Corporate Address Livermore Software Technology Corporation P. O. Box 712 Livermore, California 94551-0712 Support Addresses LSTC 7374 Las Positas Road Livermore, California 94551 Tel: 925-449-2500 ♦ Fax: 925-449-2507 Email: sales@lstc.com Website: www.lstc.com Disclaimer LSTC 1740 West Big Beaver Road Suite 100 Troy, Michigan 48084 Tel: 248-649-4728 ♦ Fax: 248-649-6328 Copyright © 1992-2017 Livermore Software Technology Corporation. All Rights Reserved. LS-DYNA®, LS-OPT® and LS-PrePost® are registered trademarks of Livermore Software Technology Corporation in the United States. All other trademarks, product names and brand names belong to their respective owners. LSTC reserves the right to modify the material contained within this manual without prior notice. The information and examples included herein are for illustrative purposes only and are not intended to be exhaustive or all-inclusive. LSTC assumes no liability or responsibility whatsoever for any direct of indirect damages or inaccuracies of any type or nature that could be deemed to have resulted from the use of this manual. Any reproduction, in whole or in part, of this manual is prohibited without the prior written approval of LSTC. All requests to reproduce the contents hereof should be sent to sales@lstc.com. ⎯⎯⎯⎯⎯⎯⎯⎯⎯⎯⎯⎯⎯⎯⎯⎯⎯⎯⎯ AES Licensing Terms Copyright © 2001, Dr Brian Gladman < brg@gladman.uk.net>, Worcester, UK. All rights reserved. The free distribution and use of this software in both source and binary form is allowed (with or without changes) provided that: 1.distributions of this source code include the above copyright notice, this list of conditions and the following disclaimer; 2.distributions in binary form include the above copyright notice, this list of conditions and the following disclaimer in the documentation and/or other associated materials; 3.he copyright holder's name is not used to endorse products built using this software without specific written permission. DISCLAIMER This software is provided 'as is' with no explicit or implied warranties in respect of any properties, including, but not limited to, correctness and fitness for purpose. This file contains the code for implementing the key schedule for AES (Rijndael) for block and key sizes of 16, 24, and 32 bytes. When defining an equation of state, the type of equation of state is specified by a corresponding 3-digit number in the command name, e.g., *EOS_004, or equivalently, by it’s more descriptive designation, e.g., *EOS_GRUNEISEN. The equations of state can be used with a subset of the materials that are available for solid elements; see the MATERIAL MODEL REFERENCE TABLES in the beginning of the *MAT section of this Manual. *EOS_015 is linked to the type 2 thick shell element and can be used to model engine gaskets. The meaning associated with particular extra history variables for a subset of material models and equations of state are tabulated at http://www.dynasupport.com/howtos- /material/history-variables. The first three extra history variables when using an equation of state are (1) internal energy, (2) pressure due to bulk viscosity, and (3) the element volume from the previous time step. TYPE 1: *EOS_LINEAR_POLYNOMIAL TYPE 2: *EOS_JWL TYPE 3: *EOS_SACK_TUESDAY TYPE 4: *EOS_GRUNEISEN TYPE 5: *EOS_RATIO_OF_POLYNOMIALS TYPE 6: *EOS_LINEAR_POLYNOMIAL_WITH_ENERGY_LEAK TYPE 7: *EOS_IGNITION_AND_GROWTH_OF_REACTION_IN_HE TYPE 8: *EOS_TABULATED_COMPACTION TYPE 9: *EOS_TABULATED TYPE 10: *EOS_PROPELLANT_DEFLAGRATION TYPE 11: *EOS_TENSOR_PORE_COLLAPSE TYPE 12: *EOS_IDEAL_GAS TYPE 14: *EOS_JWLB TYPE 15: *EOS_GASKET *EOS_MIE_GRUNEISEN TYPE 19: *EOS_MURNAGHAN TYPE 21-30: *EOS_USER_DEFINED An additional option TITLE may be appended to all the *EOS keywords. If this option is used then an additional line is read for each section in 80a format which can be used to describe the equation of state. At present LS-DYNA does not make use of the title. Inclusion of title simply gives greater clarity to input decks. Definitions and Conventions In order to prescribe the boundary and/or initial thermodynamic condition, manual computations are often necessary. Conventions or definitions must be established to simplify this process. Some basic variables are defined in the following. Since many of these variables have already been denoted by different symbols, the notations used here are unique in this section only! They are presented to only clarify their usage. A corresponding SI unit set is also presented as an example. First consider a few volumetric parameters since they are a measure of compression (or expansion). Volume: Mass: 𝑉 ≈ (m3) 𝑀 ≈ (Kg) Current specific volume (per mass): Reference specific volume: Relative volume: 𝜐 = = ≈ ( 𝑚3 Kg ) 𝜐0 = 𝑉0 = 𝜌0 ≈ ( 𝑚3 Kg ) 𝜐𝑟 = 𝑉0 = ) (𝑉 𝑀⁄ (𝑉0 𝑀⁄ ) = 𝜐0 = 𝜌0 Current normalized volume increment: 𝑑𝜐 = 𝜐 − 𝜐0 = 1 − 𝜐𝑟 = 1 − 𝜌0 𝜇 = 𝜐𝑟 − 1 = 𝜐0 − 𝜐 = − 𝑑𝜐 = 𝜌0 − 1 Sometimes another volumetric parameter is used: 𝜌0 𝜐0 𝜂 = = Thus, the relation between 𝜇 and 𝜂 is, 𝜇 = 𝜐0 − 𝜐 = 𝜂 − 1 The following table summarizes these volumetric parameters. VARIABLES COMPRESSION NO LOAD EXPANSION 𝜐𝑟 = 𝜐0 = 𝜌0 𝜂 = 𝜐𝑟 = 𝜐0 = 𝜌0 𝜇 = 𝜐𝑟 − 1 = 𝜂 − 1 < 1 > 1 > 0 V0 – Initial Relative Volume 1 1 0 > 1 < 1 < 0 There are 3 definitions of density that must be distinguished from each other: 𝜌0 = 𝜌ref = Density at nominal reference ⁄ state, usually non-stress or non-deformed state. 𝜌∣𝑡=0 = Density at time 0 𝜌 = Current density Recalling the current relative volume 𝜐𝑟 = 𝜌0 = 𝜐0 , at time = 0 the relative volume is 𝜐𝑟0 = 𝜐𝑟|𝑡=0 = 𝜌0 𝜌∣𝑡=0 = 𝜐|𝑡=0 𝜐0 . Generally, the V0 input parameter in an *EOS card refers to this 𝜐𝑟0. 𝜌0 is generally the density defined in the *MAT card. Hence, if a material is mechanically compressed at (𝜐0 ≠ 𝑉0). The “reference” state is a unique state with respect to which the material stress tensor is computed. Therefore 𝜐0 is very critical in computing the pressure level in a material. Incorrect choice of 𝜐0 would lead to incorrect pressure computed. In general, 𝜐0 is chosen such that at zero compression or expansion, the material should be in equilibrium with its ambient surrounding. In many of the equations shown in the EOS section, 𝜇 is frequently used as a measure of compression (or expansion). However, the users must clearly distinguish between 𝜇 and 𝜐𝑟0. E0 – Internal Energy Internal energy represents component) of a system. One definition for internal energy is thermal energy state the (temperature dependent 𝐸 = 𝑀𝐶𝑣𝑇 ≈ (Joule) Note that the capital “𝐸” here is the absolute internal energy. It is not the same as that used in the subsequent *EOS keyword input, or some equations shown for each *EOS card. This internal energy is often defined with respect to a mass or volume unit. Internal energy per unit mass (also called specific internal energy): 𝑒 = = 𝐶𝑉𝑇 ≈ ( Joule Kg ) Internal energy per unit current volume: 𝑒𝑉 = 𝐶𝑉𝑇 = 𝜌𝐶𝑉𝑇 = 𝐶𝑉𝑇 ≈ ( Joule m3 = m2) Internal energy per unit reference volume: 𝑒𝑉0 = 𝑉0 𝐶𝑣𝑇 = 𝜌0𝐶𝑣𝑇 = 𝐶𝑣𝑇 𝜐0 ≈ ( Joule m3 = m2) 𝑒𝑉0 typically refers to the capital “E” shown in some equations under this “EOS” section. Hence the initial “internal energy per unit reference volume”, E0, a keyword input parameter in the *EOS section can be computed from To convert from 𝑒𝑉0 to 𝑒𝑉, simply divide 𝑒𝑉0 by 𝜐𝑟 𝑒𝑉0∣ 𝑡=0 = 𝜌0𝐶𝑉𝑇|𝑡=0 𝑒𝑉 = 𝜌𝐶𝑉𝑇 = [𝜌0𝐶𝑉𝑇] 𝜌0 = 𝑒𝑉0 𝜐𝑟 A thermodynamic state of a homogeneous material, not undergoing any chemical reactions or phase changes, may be defined by two state variables. This relation is generally called an equation of state. For example, a few possible forms relating pressure to two other state variables are 𝑃 = 𝑃(𝜌, 𝑇) = 𝑃(𝜐, 𝑒) = 𝑃(𝜐𝑟, 𝑒𝑉) = 𝑃(𝜇, 𝑒𝑉0) The last equation form is frequently used to compute pressure. The EOS for solid phase materials is sometimes partitioned into 2 terms, a cold pressure and a thermal pressure 𝑃 = 𝑃𝑐(𝜇) + 𝑃𝑇(𝜇, 𝑒𝑉0) 𝑃𝑐(𝜇) is the cold pressure hypothetically evaluated along a 0-degree-Kelvin isotherm. This is sometimes called a 0-K pressure-volume relation or cold compression curve. 𝑃𝑇(𝜇, 𝑒𝑉0) is the thermal pressure component that depends on both volumetric compression and thermal state of the material. Different forms of the EOS describe different types of materials and how their volumetric compression (or expansion) behaviors. The coefficients for each EOS model come from data-fitting, phenomenological descriptions, or derivations based on classical thermodynamics, etc. Linear Compression In low pressure processes, pressure is not significantly affected by temperature. When volumetric compression is within an elastic linear deformation range, a linear bulk modulus may be used to relate volume changes to pressure changes. Recalling the definition of an isotropic bulk modulus is [Fung 1965], This may be rewritten as Δ𝜐 = − . 𝑃 = 𝐾 [− Δ𝜐 ] = 𝐾𝜇. The bulk modulus, 𝐾, thus is equivalent to 𝐶1 in *EOS_LINEAR_POLYNOMIAL when all other coefficients are zero. This is a simplest form of an EOS. To initialize a pressure for such a material, only 𝜐𝑟0 must be defined. Initial Conditions In general, a thermodynamic state must be defined by two state variables. The need to specify 𝜐𝑟0 and/or 𝑒𝑉0∣ depends on the form of the EOS chosen. The user should review the equation term-by-term to establish what parameters to be initialized. 𝑡=0 or 𝜐𝑟0. Consider two possibilities (1) 𝑇|𝑡=0 is defined or assumption on either 𝑒𝑉0∣ assumed from which 𝑒𝑉0∣ may be computed, or (2) 𝜌∣𝑡=0 is defined or assumed from 𝑡=0 which 𝜐𝑟0 may be obtained. 𝑡=0 When to Use EOS For small strains considerations, a total stress tensor may be partitioned into a deviatoric stress component and a mechanical pressure. 𝜎𝑖𝑗 = 𝜎𝑖𝑗 ′ + 𝜎𝑘𝑘 𝛿𝑖𝑗 = 𝜎𝑖𝑗 ′ − 𝑃𝛿𝑖𝑗 𝑃 = − 𝜎𝑘𝑘 The pressure component may be written from the diagonal stress components. Note that 𝜎𝑘𝑘 3 = [𝜎11+𝜎22+𝜎33] is positive in tension while P is positive in compression. Similarly, the total strain tensor may be partitioned into a deviatoric strain component (volume-preserving deformation) and a volumetric deformation. 𝜀𝑘𝑘 𝜀𝑘𝑘 3 is called the mean normal strain, and 𝜀𝑘𝑘 is called the dilatation or volume 𝜀𝑖𝑗 = 𝜀𝑖𝑗 ′ + 𝛿𝑖𝑗 where strain (change in volume per unit initial volume) 𝜀𝑘𝑘 = 𝑉 − 𝑉0 𝑉0 ′ ) as a Roughly speaking, a typical convention may refer to the relation 𝜎𝑖𝑗 “constitutive equation”, and 𝑃 = 𝑓 (𝜇, 𝑒𝑉0) as an EOS. The use of an EOS may be omitted only when volumetric deformation is very small, and |𝑃| A ∣𝜎𝑖𝑗 ′ = 𝑓 (𝜀𝑖𝑗 ′ ∣. A Note About Contact When Using an Equation of State When a part includes an equation of state, it is important that the initial geometry of that part not be perturbed by the contact algorithm. Such perturbation can arise due to initial penetrations in the contact surfaces but can usually be avoided by setting the variable IGNORE to 1 or 2 in the *CONTACT input or by using a segment based contact (SOFT = 2). This is Equation of state Form 1. *EOS_LINEAR_POLYNOMIAL Purpose: thermodynamic state of the material by defining E0 and V0 below. Define coefficients for a linear polynomial EOS, and initialize the Card 1 1 Variable EOSID Type A8 Card 2 Variable 1 E0 Type F VARIABLE EOSID C0 C1 ⋮ C6 E0 V0 3 C1 F 3 4 C2 F 4 5 C3 F 5 6 C 4 F 6 7 C5 F 7 8 C6 F 8 2 C0 F 2 V0 F DESCRIPTION Equation of state ID, a unique number or label not exceeding 8 characters must be specified. The 0th polynomial equation coefficient. The 1st polynomial equation coefficient (when used by itself, this is the elastic bulk modulus, i.e. it cannot be used for deformation that is beyond the elastic regime). ⋮ The 6th polynomial equation coefficient. Initial internal energy per unit reference volume . Initial relative volume . *EOS 1. The linear polynomial equation of state is linear in internal energy. The pressure is given by: 𝑃 = 𝐶0 + 𝐶1𝜇 + 𝐶2𝜇2 + 𝐶3𝜇3 + (𝐶4 + 𝐶5𝜇 + 𝐶6𝜇2)𝐸. 𝐶2𝜇2 is the ratio where terms of current density to reference density. 𝜌 is a nominal or reference density defined in the *MAT_NULL card. are set to zero if 𝜇 < 0, 𝜇 = − 1, and and 𝐶6𝜇2 𝜌0 𝜌0 The linear polynomial equation of state may be used to model gas with the gamma law equation of state. This may be achieved by setting: 𝐶0 = 𝐶1 = 𝐶2 = 𝐶3 = 𝐶6 = 0 and where 𝐶4 = 𝐶5 = 𝛾 − 1 𝛾 = 𝐶𝑝 𝐶𝑣 is the ratio of specific heats. Pressure for a perfect gas is then given by: 𝑝 = (𝛾 − 1) 𝜌0 𝐸 E has the unit of pressure (where 𝜌 and 𝜌) 2. When 𝐶0 = 𝐶1 = 𝐶2 = 𝐶3 = 𝐶6 = 0, it does not necessarily mean that the initial pressure is zero, 𝑃0 ≠ 𝐶0! The initial pressure depends the values of all the coefficients and on 𝜇∣𝑡=0 and 𝐸∣𝑡=0. The pressure in a material is computed from the whole equation above, 𝑃 = 𝑃(μ, 𝐸). It is always preferable to initialize the initial condition based on 𝜇∣𝑡=0 and 𝐸∣𝑡=0. The use of 𝐶0 = 𝐶1 = 𝐶2 = 𝐶3 = 𝐶6 = 0 must be done with caution as it may change the form and behavior of the material. The safest way is to use the whole EOS equation to manually check for the pressure value. For example, for ideal gas, for ideal gas, only 𝐶4 and 𝐶5 are nonzero, 𝐶4 = 𝐶5 = 𝛾 − 1 and all other coefficients 𝐶0 = 𝐶1 = 𝐶2 = 𝐶3 = 𝐶6 = 0 to satisfy the perfect gas equation form. 3. V0 and E0 defined in this card must be the same as the time-zero ordinates for the 2 load curves defined in the *BOUNDARY_AMBIENT_EOS card, if it is used. This is so that they would both consistently define the same initial state for a material. This is Equation of state Form 2. Available options are: <BLANK> AFTERBURN *EOS_JWL Card 1 1 Variable EOSID Type A8 2 A F 3 B F 4 R1 F 5 R2 F 6 OMEG F 7 E0 F 8 VO F Afterburn card. Additional card for afterburn option with OPT = 1 or 2. Card 2 1 Variable OPT Type F 2 QT F 3 T1 F 4 T2 F 5 6 7 8 Afterburn card. Additional card for afterburn option with OPT = 3. Card 2 1 Variable OPT Type F 2 Q0 F 3 QA F 4 QM 5 6 7 8 QN CONM CONL CONT F F F 1. F 1. F 1. Default none none none 0.5 1/6 VARIABLE EOSID 1-18 (EOS) DESCRIPTION Equation of state ID, a unique number or label not exceeding 8 DESCRIPTION *EOS A B R1 R2 𝐴, See equation in Remarks. 𝐵, See equation in Remarks. 𝑅1, See equation in Remarks. 𝑅2, See equation in Remarks. OMEG 𝜔, See equation in Remarks. E0 V0 OPT QT T1 T2 Q0 QA QM QN Detonation energy per unit volume and initial value for 𝐸. See equation in Remarks. Initial relative volume, which gives the initial value for 𝑉. See equation in Remarks. Afterburn option EQ.0.0: No afterburn energy (Standard EOS_JWL) EQ.1.0: Constant rate of afterburn energy added between times T1 and T2 EQ.2.0: Linearly-increasing rate of afterburn energy added between times T1 and T2 EQ.3.0: Miller’s extension for afterburn energy Afterburn energy per unit volume (OPT = 1,2) for simple afterburn Start time of energy addition for simple afterburn End time of energy addition for simple afterburn Afterburn energy per unit volume for Miller’s extension (OPT = 3) Energy release constant 𝑎 for Miller’s extension Energy release exponent 𝑚 for Miller’s extension Pressure exponent 𝑛 for Miller’s extension CONM CONL CONT Remarks: *EOS_JWL DESCRIPTION GT.0.0: Mass conversion factor from model units to calibration units for Miller’s extension LT.0.0: Use predefined factors to convert model units to published calibration units of g, cm, µs. Choices for model units are: EQ.-1.0: g, mm, ms EQ.-2.0: g, cm, ms EQ.-3.0: kg, m, s EQ.-4.0: kg, mm, ms EQ.-5.0: metric ton, mm, s EQ.-6.0: lbf-s2/in, in, s EQ.-7.0: slug, ft, s CONM.GT.0.0: Length conversion factor from model units to calibration units for Miller’s extension CONM.LT.0.0: Ignored CONM.GT.0.0: Time conversion factor from model units to calibration units for Miller’s extension CONM.LT.0.0: Ignored The JWL equation of state defines the pressure as 𝑝 = 𝐴 (1 − 𝑅1𝑉 ) 𝑒−𝑅1𝑉 + 𝐵 (1 − 𝑅2𝑉 ) 𝑒−𝑅2𝑉 + 𝜔𝐸 , and is usually used for detonation products of high explosives. A, B, and E0 have units of pressure. R1, R2, OMEG, and V0 are dimensionless. It is recommended that a unit system of gram, centimeter, microsecond be used when a model includes high explosive(s). In this consistent unit system, pressure is in Mbar. When this equation of state is used with *MAT_HIGH_EXPLOSIVE_BURN in which the variable BETA is set to 0 or 2, the absolute value of the history variable labeled as “effective plastic strain” is the explosive lighting time. This lighting time takes into account shadowing if invoked . There are four additional history variables for the JWL equation of state. Those history variables are internal energy, bulk viscosity in units of pressure, volume, and burn fraction, respectively. To output the history variables, set the variable NEIPH in *DATABASE_EXTENT_BINARY. The AFTERBURN option allows the addition of afterburn energy 𝑄 to the calculation of pressure by replacing 𝐸 in the above equation with (𝐸 + 𝑄), i.e. the last term on the right-hand side becomes 𝜔(𝐸 + 𝑄) The simple afterburn option adds the energy at a constant rate (OPT = 1) or a linearly- increasing rate (OPT = 2) between times T1 and T2 such that the total energy added per unit volume at time T2 is the specified energy QT. For the Miller’s extension model (OPT = 3), the afterburn energy is added via a time- dependent growth term 𝑑𝜆 𝑑𝑡 = 𝑎(1 − 𝜆)𝑚𝑝𝑛, 𝑄 = 𝜆𝑄0 Here, 𝑚, 𝑛, and 𝜆 are dimensionless, with 𝜆 a positive fraction less than 1.0. The parameter 𝑎 has units consistent with this growth equation, and 𝑄0 has units of pressure. The values for 𝑄0, 𝑎, 𝑚, 𝑛 published by Miller and Guirguis (1993) are calibrated in the units of g, cm, µs, with the consistent pressure unit of Mbar, though in principle any consistent set of units may be used for calibration. The factors CONM, CONL, and CONT convert the unit system of the model being analyzed to the calibration unit system in which the Miller’s extension parameters are specified, e.g. a mass value in model units may be multiplied by CONM to obtain the corresponding value in calibration units. These conversion factors allow consistent evaluation of the growth equation in the calibrated units. For user convenience, predefined conversion factors are provided for converting various choices for the model units system to the calibration unit system used by Miller and Guirguis. The AFTERBURN option introduces an additional 5th history variable that records the added afterburn energy 𝑄 for simple afterburn (OPT = 1,2), but contains the growth term 𝜆 when using the Miller’s extension model (OPT = 3). This is Equation of state Form 3. *EOS_SACK_TUESDAY Card 1 1 Variable EOSID Type A8 2 A1 F 3 A2 F 4 A3 F 5 B1 F 6 B2 F 7 E0 F 8 V0 F VARIABLE EOSID DESCRIPTION Equation of state ID, a unique number or label not exceeding 8 characters must be specified. Ai, Bi Constants in the equation of state E0 V0 Initial internal energy Initial relative volume Remarks: The Sack equation of state defines pressure as 𝑝 = 𝐴3 𝑉𝐴1 𝑒−𝐴2𝑉 (1 − 𝐵1 ) + 𝐵2 𝐸 and is used for detonation products of high explosives. This is Equation of state Form 4. *EOS Card 1 1 Variable EOSID Type A8 Card 2 Variable 1 V0 Type F VARIABLE EOSID 2 C F 2 3 S1 F 3 4 S2 F 4 5 S3 F 5 6 GAMAO F 6 7 A F 7 8 E0 F 8 DESCRIPTION Equation of state ID, a unique number or label not exceeding 8 characters must be specified. C, Si, GAMMA0 Constants in the equation of state First order volume correction coefficient Initial internal energy Initial relative volume A E0 V0 Remarks: The Gruneisen equation of state with cubic shock-velocity as a function of particle- velocity 𝑣𝑠(𝑣𝑝) defines pressure for compressed materials as 𝜌0𝐶2𝜇[1 + (1 − )𝜇 − 𝑎 𝜇2] 𝑝 = 𝛾0 𝜇2 𝜇 + 1 − 𝑆3 𝜇3 (𝜇 + 1)2] [1 − (𝑆1 − 1)𝜇 − 𝑆2 and for expanded materials as 2 + (𝛾0 + 𝑎𝜇)𝐸. 𝑝 = 𝜌0𝐶2𝜇 + (𝛾0 + 𝑎𝜇)𝐸. where C is the intercept of the 𝑣𝑠(𝑣𝑝) curve (in velocity units); S1, S2, and S3 are the unitless coefficients of the slope of the 𝑣𝑠(𝑣𝑝) curve; γ 0 is the unitless Gruneisen gamma; a is the unitless, first order volume correction to γ 0; and 𝜇 = 𝜌0 − 1. This is Equation of state Form 5. *EOS Card 1 1 2 3 4 5 6 7 8 Variable EOSID Type A8 Card 2 1 2 3 4 5 6 7 8 Variable A10 Type F A11 F A12 F A13 F Card 3 1 2 3 4 5 6 7 8 Variable A20 Type F A21 F A22 F A23 F Card 4 1 2 3 4 5 6 7 8 Variable A30 Type F A31 F A32 F A33 F Card 5 1 2 3 4 5 6 7 8 Variable A40 Type F A41 F A42 F A43 Card 6 1 2 3 4 5 6 7 8 Variable A50 Type F A51 F A52 F A53 F Card 7 1 2 3 4 5 6 7 8 Variable A60 Type F A61 F A62 F A63 F Card 8 1 2 3 4 5 6 7 8 Variable A70 Type F A71 F A72 F A73 F Card 9 1 2 3 4 5 6 7 8 Variable A14 Type F A24 F Card 10 1 2 3 4 5 6 7 8 Variable ALPH Type F BETA F E0 F V0 F VARIABLE EOSID DESCRIPTION Equation of state ID, a unique number or label not exceeding 8 characters must be specified. Aij Polynomial coefficients VARIABLE DESCRIPTION α β Initial internal energy Initial relative volume ALPHA BETA E0 V0 Remarks: The ratio of polynomials equation of state defines the pressure as where 𝑝 = 𝐹1 + 𝐹2𝐸 + 𝐹3𝐸2 + 𝐹4𝐸3 𝐹5 + 𝐹6𝐸 + 𝐹7𝐸2 (1 + 𝛼𝜇) 𝐹𝑖 = ∑ 𝐴𝑖𝑗𝜇𝑗 𝑗=0 , 𝑛 = { 𝑖 < 3 𝑖 ≥ 3 𝜌0 ′ = 𝐹1 + 𝛽𝜇2. By setting coefficient 𝐴10 = 1.0, In expanded elements 𝐹1 is replaced by 𝐹1 the delta-phase pressure modeling for this material will be initiated. The code will reset it to 0.0 after setting flags. − 1 𝜇 = *EOS_LINEAR_POLYNOMIAL_WITH_ENERGY_LEAK This is Equation of state Form 6. Define coefficients for a linear polynomial EOS, and initialize the Purpose: thermodynamic state of the material by defining E0 and V0 below. Energy deposition is prescribed via a curve. Card 1 1 Variable EOSID Type A8 Card 2 Variable 1 E0 Type F VARIABLE EOSID 4 C2 F 4 5 C3 F 5 6 C4 F 6 7 C5 F 7 8 C6 F 8 2 C0 F 2 V0 F 3 C1 F 3 LCID I DESCRIPTION Equation of state ID, a unique number or label not exceeding 8 characters must be specified. Ci E0 V0 Constants in the equation of state Initial internal energy Initial relative volume LCID Load curve ID defining the energy deposition rate. Remarks: This polynomial equation of state, linear in the internal energy per initial volume, 𝐸, is given by 𝑝 = 𝐶0 + 𝐶1𝜇 + 𝐶2𝜇2 + 𝐶3𝜇3 + (𝐶4 + 𝐶5𝜇 + 𝐶6𝜇2)𝐸 in which 𝐶1, 𝐶2, 𝐶3, 𝐶4, 𝐶5, and 𝐶6 are user defined constants and where 𝑉 is the relative volume. In expanded elements, we set the coefficients of 𝜇2 to zero, i.e., − 1 . 𝜇 = Internal energy, 𝐸, is increased according to an energy deposition rate versus time curve whose ID is defined in the input. 𝐶2 = 𝐶6 = 0 *EOS_IGNITION_AND_GROWTH_OF_REACTION_IN_HE This is Equation of state Form 7. Card 1 1 Variable EOSID Type A8 Card 2 Variable 1 R2 Type F Card 3 1 2 A F 2 R3 F 2 3 B F 3 R5 F 3 4 5 6 XP1 XP2 FRER F 5 F 6 7 G F 7 8 R1 F 8 FMXIG FREQ GROW1 EM F 5 F 6 F 7 F 8 F 4 R6 F 4 Variable AR1 ES1 CVP CVR EETAL CCRIT ENQ TMP0 Type F Card 4 1 F 2 F 3 F 4 F 5 F 6 F 7 F 8 Variable GROW2 AR2 ES2 EN FMXGR FMNGR Type F F F F F F VARIABLE EOSID DESCRIPTION Equation of state ID, a unique number or label not exceeding 8 characters must be specified. A B Product JWL constant Product JWL constant XP1 Product JWL constant VARIABLE DESCRIPTION XP2 FRER G R1 R2 R3 R5 R6 Product JWL constant Constant in ignition term of reaction equation 𝜔𝐶𝑣 of product Unreacted JWL constant Unreacted JWL constant 𝜔𝐶𝑣 of unreacted explosive Unreacted JWL constant Unreacted JWL constant FMXIG Maximum F for ignition term FREQ Constant in ignition term of reaction equation GROW1 Constant in growth term of reaction equation EM AR1 ES1 CVP CVR Constant in growth term of reaction equation Constant in growth term of reaction equation Constant in growth term of reaction equation Heat capacity of reaction products Heat capacity of unreacted HE EETAL Constant in ignition term of reaction equation CCRIT Constant in ignition term of reaction equation ENQ TMP0 Heat of reaction Initial temperature (°K) GROW2 Constant in completion term of reaction equation AR2 ES2 EN Constant in completion term of reaction equation Constant in completion term of reaction equation Constant in completion term of reaction equation VARIABLE DESCRIPTION FMXGR Maximum F for growth term FMNGR Maximum F for completion term Remarks: Equation of State Form 7 is used to calculate the shock initiation (or failure to initiate) and detonation wave propagation of solid high explosives. It should be used instead of the ideal HE burn options whenever there is a question whether the HE will react, there is a finite time required for a shock wave to build up to detonation, and/or there is a finite thickness of the chemical reaction zone in a detonation wave. At relatively low initial pressures (<2-3 GPa), this equation of state should be used with material type 10 for accurate calculations of the unreacted HE behavior. At higher initial pressures, material type 9 can be used. A JWL equation of state defines the pressure in the unreacted explosive as 𝑃𝑒 = 𝑟1𝑒−𝑟5𝑉𝑒 + 𝑟2𝑒−𝑟6𝑉𝑒 + 𝑟3 𝑇𝑒 𝑉𝑒 , (𝑟3 = 𝜔𝑒Cvr) where 𝑉𝑒 and 𝑇𝑒 are the relative volume and temperature, respectively, of the unreacted explosive. Another JWL equation of state defines the pressure in the reaction products as 𝑃𝑝 = 𝑎𝑒−𝑥𝑝1𝑉𝑝 + 𝑏𝑒−𝑥𝑝2𝑉𝑝 + 𝑔𝑇𝑝 𝑉𝑝 , (𝑔 = 𝜔𝑝Cvp) where 𝑉𝑝 and 𝑇𝑝 are the relative volume and temperature, respectively, of the reaction products. As the chemical reaction converts unreacted explosive to reaction products, these JWL equations of state are used to calculate the mixture of unreacted explosive and reaction products defined by the fraction reacted F(F = O implies no reaction, F = 1 implies complete reaction). The temperatures and pressures are assumed to be equal (𝑇𝑒 = 𝑇𝑝, 𝑝𝑒 = 𝑝𝑝) and the relative volumes are additive, i.e., 𝑉 = (1 − 𝐹)𝑉𝑒 + 𝐹𝑉𝑝 The chemical reaction rate for conversion of unreacted explosive to reaction products consists of three physically realistic terms: an ignition term in which a small amount of explosive reacts soon after the shock wave compresses it; a slow growth of reaction as this initial reaction spreads; and a rapid completion of reaction at high pressure and temperature. The form of the reaction rate equation is Ignition ⏞⏞⏞⏞⏞⏞⏞⏞⏞⏞⏞⏞⏞⏞⏞⏞⏞⏞⏞⏞⏞⏞⏞ −1 − 1 − CCRIT)EETAL = FREQ × (1 − 𝐹)FRER(𝑉𝑒 Growth ⏞⏞⏞⏞⏞⏞⏞⏞⏞⏞⏞⏞⏞⏞⏞ + GROW1 × (1 − 𝐹)ES1𝐹AR1𝑝EM 𝜕𝐹 𝜕𝑡 + GROW2 × (1 − 𝐹)ES2𝑓 AR2𝑝EN ⏟⏟⏟⏟⏟⏟⏟⏟⏟⏟⏟⏟⏟⏟⏟ Completion The ignition rate is set equal to zero when 𝐹 ≥ FMXIG, the growth rate is set equal to zero when 𝐹 ≥ FMXGR, and the completion rate is set equal to zero when 𝐹 ≤ FMNGR. Details of the computational methods and many examples of one and two dimensional shock initiation and detonation wave calculation can be found in the references (Cochran and Chan [1979], Lee and Tarver [1980]). Unfortunately, sufficient experimental data has been obtained for only two solid explosives to develop very reliable shock initiation models: PBX-9504 (and the related HMX-based explosives LX- 14,LX-10,LX-04, etc.) and LX-17 (the insensitive TATB-based explosive). Reactive flow models have been developed for other explosives (TNT, PETN, Composition B, propellants, etc.) but are based on very limited experimental data. When this EOS is used with *MAT_009, history variables 4, 7, 9, and 10 are temperature, burn fraction, 1/𝑉𝑒, and 1/𝑉𝑝, respectively. When used with *MAT_010, those histories variables are incremented by 1, i.e., history variables 5, 8, 10, and 11 are temperature, burn fraction, 1/𝑉𝑒, and 1/𝑉𝑝, respectively. See NEIPH in *DATABASE_EXTENT_BI- NARY if these output variables are desired in the databases for post-processing. *EOS_TABULATED_COMPACTION This is Equation of state Form 8. Card 1 1 2 Variable EOSID GAMA Type A8 F 3 E0 F 4 V0 F 5 6 7 8 LCC LCT LCK I I I Parameter Card Pairs. Include one pair of the following two cards for each of VAR = 𝜀𝑣𝑖 , 𝐶𝑖, 𝑇𝑖, and 𝐾𝑖. These cards consist of four additional pairs for a total of 8 additional cards. Card 3 1 2 3 4 5 6 7 8 9 10 Variable [VAR]1 [VAR]2 [VAR]3 [VAR]4 [VAR]5 Type F F F F F Card 4 1 2 3 4 5 6 7 8 9 10 Variable [VAR]6 [VAR]7 [VAR]8 [VAR]9 [VAR]10 Type F F F F F VARIABLE EOSID DESCRIPTION Equation of state ID, a unique number or label not exceeding 8 characters must be specified. GAMA 𝛾, (unitless), see equation in Remarks. E0 V0 Initial internal energy per unit reference volume (force per unit area). Initial relative volume (unitless). VARIABLE LCC DESCRIPTION Load curve defining tabulated function 𝐶. See equation in Remarks. The abscissa values of LCC, LCT and LCK must be negative of the volumetric strain in monotonically increasing order, in contrast to the convention in EOS_9. The definition can extend into the tensile regime. LCT Load curve defining tabulated function 𝑇. See equation in Remarks. LCK Load curve defining tabulated bulk modulus. 𝜀𝑣1, 𝜀𝑣2 , …, 𝜀𝑣𝑁 Volumetric strain, ln(𝑉). The first abscissa point, EV1, must be 0.0 or positive if the curve extends into the tensile regime with subsequent points decreasing monotonically. 𝐶1, 𝐶2, …, 𝐶𝑁 𝐶(𝜀𝑉), (units = force per unit area), see equation in Remarks. 𝑇1, 𝑇2, …, 𝑇𝑁 𝑇(𝜀𝑉), (unitless), see equation in Remarks. 𝐾1, 𝐾2, …, 𝐾𝑁 Bulk unloading modulus (units = force per unit area). v6 v5 v4 v3 ε v2 v1 ln(V/V0) Figure EOS8-1. Pressure versus volumetric strain curve for Equation of state Form 8 with compaction. In the compacted states the bulk unloading modulus depends on the peak volumetric strain. Volumetric strain values should be input with correct sign (negative in compression) and in descending order. Pressure is positive in compression. VARIABLE DESCRIPTION Remarks: The tabulated compaction model is linear in internal energy. Pressure is defined by 𝑝 = 𝐶(𝜀𝑉) + 𝛾 𝑇(𝜀𝑉)𝐸 in the loading phase. The volumetric strain, 𝜀𝑉 is given by the natural logarithm of the relative volume 𝑉. Unloading occurs along the unloading bulk modulus to the pressure cutoff. The pressure cutoff, a tension limit, is defined in the material model definition. Reloading always follows the unloading path to the point where unloading began, and continues on the loading path, see Figure EOS8-1. Up to 10 points and as few as 2 may be used when defining the tabulated functions. LS-DYNA will extrapolate to find the pressure if necessary. This is Equation of state Form 9. *EOS Card 1 1 2 Variable EOSID GAMA Type A8 F 3 E0 F 4 V0 F 5 6 7 8 LCC LCT I I Parameter Card Pairs. Include one pair of the following two cards for each of VAR = 𝜀𝑉𝑖 , 𝐶𝑖, 𝑇𝑖. These cards consist of three additional pairs for a total of 6 additional cards. These cards are not required if LCC and LCT are specified. Card 2 1 2 3 4 5 6 7 8 9 10 Variable [VAR]1 [VAR]2 [VAR]3 [VAR]4 [VAR]5 Type F F F F F Card 3 1 2 3 4 5 6 7 8 9 10 Variable [VAR]6 [VAR]7 [VAR]8 [VAR]9 [VAR]10 Type F F F F F VARIABLE EOSID DESCRIPTION Equation of state ID, a unique number or label not exceeding 8 characters must be specified. GAMA 𝛾, (unitless) see equation in Remarks. E0 V0 Initial internal energy per unit reference volume (force per unit area). Initial relative volume (unitless). VARIABLE DESCRIPTION LCC LCT Load curve defining tabulated function 𝐶. See equation in Remarks. The abscissa values of LCC and LCT must increase monotonically. The definition can extend into the tensile regime. Load curve defining tabulated function 𝑇. See equation in Remarks. 𝜀𝑉1, 𝜀𝑉2, …, 𝜀𝑉𝑁 Volumetric strain, ln(𝑉), where 𝑉 is the relative volume. The first abscissa point, EV1, must be 0.0 or positive if the curve extends into the tensile regime with subsequent points decreasing monotonically. 𝐶1, 𝐶2, …, 𝐶𝑁 Tabulated points for function 𝐶 (force per unit area). 𝑇1, 𝑇2, …, 𝑇𝑁 Tabulated points for function 𝑇 (unitless). Remarks: The tabulated equation of state model is linear in internal energy. Pressure is defined by 𝑃 = 𝐶(𝜀𝑉) + 𝛾𝑇(𝜀𝑉)𝐸 The volumetric strain, 𝜀𝑉 is given by the natural logarithm of the relative volume 𝑉. Up to 10 points and as few as 2 may be used when defining the tabulated functions. LS- DYNA will extrapolate to find the pressure if necessary. *EOS_PROPELLANT_DEFLAGRATION This Equation of state (10) has been added to model airbag propellants. Card 1 1 Variable EOSID Type A8 Card 2 Variable Type Card 3 Variable 1 G F 1 R6 2 A F 2 R1 F 2 3 B F 3 R2 F 3 4 5 6 7 8 XP1 XP2 FRER F F 4 R3 F 4 5 R5 F 5 F 6 7 8 6 7 8 FMXIG FREQ GROW1 EM Type F Card 4 1 F 2 F 3 F 4 F 5 6 7 8 Variable AR1 ES1 CVP CVR EETAL CCRIT ENQ TMP0 Type F Card 5 1 F 2 F 3 F 4 F 5 6 7 8 Variable GROW2 AR2 ES2 EN FMXGR FMNGR Type F F F F F EOSID *EOS_PROPELLANT_DEFLAGRATION DESCRIPTION Equation of state ID, a unique number or label not exceeding 8 characters must be specified. A B XP1 XP2 Product JWL coefficient Product JWL coefficient Product JWL coefficient Product JWL coefficient FRER Unreacted Co-volume G R1 R2 R3 R5 R6 FMXIG FREQ Product 𝜔𝐶𝑣 Unreacted JWL coefficient Unreacted JWL coefficient Unreacted 𝜔𝐶𝑣 Unreacted JWL coefficient Unreacted JWL coefficient Initial Fraction Reacted 𝐹0 Initial Pressure 𝑃0 GROW1 First burn rate coefficient EM AR1 ES1 CVP CVR Pressure Exponent (1st term) Exponent on 𝐹 (1st term) Exponent on (1 − 𝐹) (1st term) Heat capacity 𝐶𝑣 for products Heat capacity 𝐶𝑣 for unreacted material EETAL Extra, not presently used CCRIT Product co-volume ENQ Heat of Reaction VARIABLE DESCRIPTION TMP0 Initial Temperature (298°K) GROW2 Second burn rate coefficient AR2 ES2 EN Exponent on 𝐹 (2nd term) Exponent on (1 − 𝐹) (2nd term) Pressure Exponent (2nd term) FMXGR Maximum 𝐹 for 1st term FMNGR Minimum 𝐹 for 2nd term Remarks: A deflagration (burn rate) reactive flow model requires an unreacted solid equation of state, a reaction product equation of state, a reaction rate law and a mixture rule for the two (or more) species. The mixture rule for the standard ignition and growth model [Lee and Tarver 1980] assumes that both pressures and temperatures are completely equilibrated as the reaction proceeds. However, the mixture rule can be modified to allow no thermal conduction or partial heating of the solid by the reaction product gases. For this relatively slow process of airbag propellant burn, the thermal and pressure equilibrium assumptions are valid. The equations of state currently used in the burn model are the JWL, Gruneisen, the van der Waals co-volume, and the perfect gas law, but other equations of state can be easily implemented. In this propellant burn, the gaseous nitrogen produced by the burning sodium azide obeys the perfect gas law as it fills the airbag but may have to be modeled as a van der Waal’s gas at the high pressures and temperatures produced in the propellant chamber. The chemical reaction rate law is pressure, particle geometry and surface area dependent, as are most high- pressure burn processes. When the temperature profile of the reacting system is well known, temperature dependent Arrhenius chemical kinetics can be used. Since the airbag propellant composition and performance data are company private information, it is very difficult to obtain the required information for burn rate modeling. However, Imperial Chemical Industries (ICI) Corporation supplied pressure exponent, particle geometry, packing density, heat of reaction, and atmospheric pressure burn rate data which allowed us to develop the numerical model presented here for their NaN3 + Fe2O3 driver airbag propellant. The deflagration model, its implementation, and the results for the ICI propellant are presented in [Hallquist, et.al., 1990]. The unreacted propellant and the reaction product equations of state are both of the form: 𝑝 = 𝐴𝑒−𝑅1𝑉 + 𝐵𝑒−𝑅2𝑉 + 𝜔𝐶𝑣𝑇 𝑉 − 𝑑 where 𝑝 is pressure (in Mbars), 𝑉 is the relative specific volume (inverse of relative density), 𝜔 is the Gruneisen coefficient, 𝐶𝑣 is heat capacity (in Mbars -cc/cc°K), 𝑇 is temperature in °K, 𝑑 is the co-volume, and 𝐴, 𝐵, 𝑅1 and 𝑅2 are constants. Setting 𝐴 = 𝐵 = 0 yields the van der Waal’s co-volume equation of state. The JWL equation of state is generally useful at pressures above several kilobars, while the van der Waal’s is useful at pressures below that range and above the range for which the perfect gas law holds. Additionally, setting 𝐴 = 𝐵 = 𝑑 = 0 yields the perfect gas law. If accurate values of 𝜔 and 𝐶𝑣 plus the correct distribution between “cold” compression and internal energies are used, the calculated temperatures are very reasonable and thus can be used to check propellant performance. The reaction rate used for the propellant deflagration process is of the form: ∂𝐹 ∂𝑡 = 𝑍(1 − 𝐹)𝑦𝐹𝑥𝑝𝑤 ⏟⏟⏟⏟⏟⏟⏟ 0<𝐹<𝐹limit1 + 𝑉(1 − 𝐹)𝑢𝐹𝑟𝑝𝑠 ⏟⏟⏟⏟⏟⏟⏟ 𝐹limit2<𝐹<1 where 𝐹 is the fraction reacted (𝐹 = 0 implies no reaction, 𝐹 = 1 is complete reaction), 𝑡 is time, and 𝑝 is pressure (in Mbars), 𝑟, 𝑠, 𝑢, 𝑤, 𝑥, 𝑦, 𝐹limit1 and 𝐹limit2 are constants used to describe the pressure dependence and surface area dependence of the reaction rates. Two (or more) pressure dependant reaction rates are included in case the propellant is a mixture or exhibited a sharp change in reaction rate at some pressure or temperature. Burning surface area dependencies can be approximated using the (1 − 𝐹)𝑦𝐹𝑥 terms. Other forms of the reaction rate law, such as Arrhenius temperature dependent 𝑒−𝐸 𝑅𝑇⁄ type rates, can be used, but these require very accurate temperatures calculations. Although the theoretical justification of pressure dependent burn rates at kilobar type pressures is not complete, a vast amount of experimental burn rate versus pressure data does demonstrate this effect and hydrodynamic calculations using pressure dependent burn accurately simulate such experiments. The deflagration reactive flow model is activated by any pressure or particle velocity increase on one or more zone boundaries in the reactive material. Such an increase creates pressure in those zones and the decomposition begins. If the pressure is relieved, the reaction rate decreases and can go to zero. This feature is important for short duration, partial decomposition reactions. If the pressure is maintained, the fraction reacted eventually reaches one and the material is completely converted to product molecules. The deflagration front rates of advance through the propellant calculated by this model for several propellants are quite close to the experimentally observed burn rate versus pressure curves. To obtain good agreement with experimental deflagration data, the model requires an accurate description of the unreacted propellant equation of state, either an analytical fit to experimental compression data or an estimated fit based on previous experience with similar materials. This is also true for the reaction products equation of state. The more experimental burn rate, pressure production and energy delivery data available, the better the form and constants in the reaction rate equation can be determined. Therefore, the equations used in the burn subroutine for the pressure in the unreacted propellant 𝑃𝑢 = R1 × 𝑒−R5⋅𝑉𝑢 + R2 × 𝑒−R6⋅𝑉𝑢 + R3 × 𝑇𝑢 𝑉𝑢 − FRER where 𝑉𝑢 and 𝑇𝑢 are the relative volume and temperature respectively of the unreacted propellant. The relative density is obviously the inverse of the relative volume. The pressure 𝑃𝑝 in the reaction products is given by: 𝑃𝑝 = A× 𝑒−XP1×𝑉𝑝 + B × 𝑒−XP2×𝑉𝑝 + G×𝑇𝑝 𝑉𝑝 − CCRIT As the reaction proceeds, the unreacted and product pressures and temperatures are assumed to be equilibrated (𝑇𝑢 = 𝑇𝑝 = 𝑇, 𝑃 = 𝑃𝑢 = 𝑃𝑝) and the relative volumes are additive: 𝑉 = (1 − 𝐹)𝑉𝑢 + 𝐹𝑉𝑝 where 𝑉 is the total relative volume. Other mixture assumptions can and have been used in different versions of DYNA2D/3D. The reaction rate law has the form: 𝜕𝐹 𝜕𝑡 = GROW1 × (𝑃 + FREQ)EM(𝐹 + FMXIG)AR1(1 − 𝐹 + FMIXG)ES1 + GROW2 × (𝑃 + FREQ)EN(𝐹 + FMIXG)AR2(1 − 𝐹 + FMIXG)ES2 If 𝐹 exceeds FMXGR, the GROW1 term is set equal to zero, and, if 𝐹 is less than FMNGR, the GROW2 term is zero. Thus, two separate (or overlapping) burn rates can be used to describe the rate at which the propellant decomposes. This equation of state subroutine is used together with a material model to describe the propellant. In the airbag propellant case, a null material model (type #10) can be used. Material type #10 is usually used for a solid propellant or explosive when the shear modulus and yield strength are defined. The propellant material is defined by the material model and the unreacted equation of state until the reaction begins. The calculated mixture states are used until the reaction is complete and then the reaction product equation of state is used. The heat of reaction, ENQ, is assumed to be a constant and the same at all values of 𝐹 but more complex energy release laws could be implemented. History variables 4 and 7 are temperature and burn fraction, respectively. See NEIPH in *DATABASE_EXTENT_BINARY if these output variables are desired in the databases for post-processing. This is Equation of state Form 11. *EOS Card 1 1 2 3 4 5 Variable EOSID NLD NCR MU1 MU2 6 IE0 7 EC0 8 Type A8 F F F F F F DESCRIPTION Equation of state ID, a unique number or label not exceeding 8 characters must be specified. Virgin loading load curve ID Completely crushed load curve ID Excess Compression required before any pores can collapse Excess Compression point where the Virgin Loading Curve and the Completely Crushed Curve intersect Initial Internal Energy Initial Excess Compression VARIABLE EOSID NLD NCR MU1 MU2 IE0 EC0 Remarks: The pore collapse model described in the TENSOR manual [23] is no longer valid and has been replaced by a much simpler method. This is due in part to the lack of experimental data required for the more complex model. It is desired to have a close approximation of the TENSOR model in the DYNA code to enable a quality link between them. The TENSOR model defines two curves, the virgin loading curve and the completely crushed curve as shown in Figure EOS11-1 also defines the excess compression point required for pore collapse to begin, 𝜇1, and the excess compression point required to completely crush the material, 𝜇2. From this data and the maximum excess compression the material has attained, 𝑢max, the pressure for any excess compression, 𝜇, can be determined. 1.0 .8 .6 .4 .2 ( ) Virgin loading curve Completely crushed curve Partially crushed curve .04 .08 .12 .16 .20 Excess Compression Figure EOS11-1. Pressure versus compaction curve Unloading occurs along the virgin loading curve until the excess compression surpasses 𝜇1. After that, the unloading follows a path between the completely crushed curve and the virgin loading curve. Reloading will follow this curve back up to the virgin loading curve. Once the excess compression exceeds 𝜇2, then all unloading will follow the completely crushed curve. For unloading between 𝜇1 and a partially𝜇2 crushed curve is determined by the relation: where 𝑝pc(𝜇) = 𝑝cc [ 𝜇𝑎 ⏞⏞⏞⏞⏞⏞⏞⏞⏞⏞⏞ (1 + 𝜇𝐵)(1 + 𝜇) − 1] 1 + 𝜇max . 𝜇𝐵 = 𝑃cc −1(𝑃max) and the subscripts “pc” and “cc” refer to the partially crushed and completely crushed states, respectively. This is more readily understood in terms of the relative volume, 𝑉. 𝑉 = 1 + 𝜇 𝑃pc(𝑉) = 𝑃cc ( 𝑉𝐵 𝑉min 𝑉) This representation suggests that for a fixed 𝑉min = 𝜇max + 1 the partially crushed curve will separate linearly from the completely crushed curve as 𝑉 increases to account for pore recovery in the material. The bulk modulus 𝐾 is determined to be the slope of the current curve times one plus the excess compression 𝐾 = ∂𝑃 ∂𝜇 (1 + 𝜇) The slope ∂𝑃 ∂𝜇 for the partially crushed curve is obtained by differentiation as: 𝜕𝑝pc 𝜕𝜇 = 𝜕𝑝cc 𝜕𝑥 ∣ 𝑥= (1+𝜇𝑏)(1+𝜇) 1+𝜇max −1 ( 1 + 𝜇𝑏 1 + 𝜇max ) Simplifying, where 𝐾 = ∂𝑃cc ∂𝜇𝑎 ∣ μa (1 + 𝜇𝑎) 𝜇𝑎 = (1 + 𝜇𝐵)(1 + 𝜇) (1 + 𝜇max) − 1. The bulk sound speed is determined from the slope of the completely crushed curve at the current pressure to avoid instabilities in the time step. The virgin loading and completely crushed curves are modeled with monotonic cubic- splines. An optimized vector interpolation scheme is then used to evaluate the cubic- splines. The bulk modulus and sound speed are derived from a linear interpolation on the derivatives of the cubic-splines. *EOS_IDEAL_GAS Purpose: This is equation of state form 12 for modeling ideal gas. It is an alternate approach to using *EOS_LINEAR_POLYNOMIAL with C4 = C5 = (𝛾 − 1) to model ideal gas. This has a slightly improved energy accounting algorithm. Card 1 1 2 3 Variable EOSID CV0 CP0 4 CL F 4 5 CQ F 5 6 T0 F 6 7 V0 F 7 8 VCO F 8 F 2 F 3 Type A8 Card 2 1 Variable ADIAB Type F VARIABLE EOSID CV0 CP0 CL CQ T0 V0 DESCRIPTION Equation of state ID, a unique number or label not exceeding 8 characters must be specified. Nominal constant-volume specific heat coefficient (at STP) Nominal constant-pressure specific heat coefficient (at STP) Linear coefficient for the variations of 𝐶𝑣 and 𝐶𝑝versus 𝑇. Quadratic coefficient for the variations of 𝐶𝑣 and 𝐶𝑝 versus 𝑇. Initial temperature Initial relative volume VCO Van der Waals covolume ADIAB Adiabatic flag: EQ.0.0: off EQ.1.0: on; ideal gas follows adiabatic law 1. The pressure in the ideal gas law is defined as *EOS 𝑝 = 𝜌(𝐶𝑝 − 𝐶𝑣)𝑇 𝐶𝑝 = 𝐶𝑝0 + 𝐶𝐿𝑇 + 𝐶𝑄𝑇2 𝐶𝑣 = 𝐶𝑣0 + 𝐶𝐿𝑇 + 𝐶𝑄𝑇2 where 𝐶𝑝 and 𝐶𝑣 are the specific heat capacities at constant pressure and at constant volume, respectively. 𝜌 is the density. The relative volume is defined as 𝜐𝑟 = 𝑉0 = ) (𝑉 𝑀⁄ ) (𝑉0 𝑀⁄ = 𝜐0 = 𝜌0 where 𝜌0 is a nominal or reference density defined in the *MAT_NULL card. The initial pressure can then be manually computed as 𝑃|𝑡=0 = 𝜌∣𝑡=0(𝐶𝑃 − 𝐶𝑉)𝑇|𝑡=0 𝜌∣𝑡=0 = { 𝑃|𝑡=0 = { 𝜌0 𝜐𝑟|𝑡=0 𝜌0 𝜐𝑟|𝑡=0 } } (𝐶𝑃 − 𝐶𝑉)𝑇|𝑡=0 The initial relative volume, 𝜐𝑟|𝑡=0 (V0), initial temperature, 𝑇|𝑡=0(T0), and heat capacity information are defined in the *EOS_IDEAL_GAS input. Note that the “reference” density is typically a density at a non-stressed or nominal stress state. The initial pressure should always be checked manually against simula- tion result. 2. With adiabatic flag on, the adiabatic state is conserved, but extact internal energy conservation is scarified. 3. The ideal gas model is good for low density gas only. Deviation from the ideal gas behavior may be indicated by the compressibility factor defined as 𝑍 = 𝑃𝜐 𝑅𝑇 When 𝑍 deviates from 1, the gas behavior deviates from ideal. 4. V0 and T0 defined in this card must be the same as the time-zero ordinates for the 2 load curves defined in the *BOUNDARY_AMBIENT_EOS card, if it is used. This is so that they both would consistently define the same initial state for a material. *EOS_JWLB This is Equation of state Form 14. The JWLB (Jones-Wilkens-Lee-Baker) equation of state, developed by Baker [1991] and further described by Baker and Orosz [1991], describes the high pressure regime produced by overdriven detonations while retaining the low pressure expansion behavior required for standard acceleration modeling. The derived form of the equation of state is based on the JWL form due to its computational robustness and asymptotic approach to an ideal gas at high expansions. Additional exponential terms and a variable Gruneisen parameter have been added to adequately describe the high-pressure region above the Chapman-Jouguet state. Card 1 1 Variable EOSID Type A8 Card 2 Variable 1 R1 Type F Card 3 1 2 A1 F 2 R2 F 2 3 A2 F 3 R3 F 3 4 A3 F 4 R4 F 4 5 A4 F 5 R5 F 5 Variable AL1 AL2 AL3 AL4 AL5 Type F Card 4 1 F 2 F 3 F 4 F 5 Variable BL1 BL2 BL3 BL4 BL5 Type F F F F F 6 A5 F 6 7 8 7 8 6 7 8 6 7 Card 5 1 2 3 4 5 6 7 8 Variable RL1 RL2 RL3 RL4 RL5 Type F Card 6 Variable Type 1 C I F 2 OMEGA F F 3 E F F 4 V0 F F 5 6 7 8 VARIABLE EOSID DESCRIPTION Equation of state ID, a unique number or label not exceeding 8 characters must be specified. Ai, Ri, Ali, BLi, C, OMEGA Equation of state coefficients 𝐴𝑖, 𝑅𝑖, 𝐴𝜆𝑖, 𝐵𝜆𝑖, 𝑅𝜆𝑖, 𝐶, 𝜔 respectively. See below. C Equation of state coefficient, see below. OMEGA Equation of state coefficient, see below. E V0 Energy density per unit initial volume Initial relative volume. Remarks: The JWLB equation-of-state defines the pressure as 𝑝 = ∑ 𝐴𝑖 𝑖=1 (1 − 𝑅𝑖𝑉 ) 𝑒−𝑅𝑖𝑉 + 𝜆𝐸 + 𝐶 (1 − ) 𝑉−(𝜔+1) 𝜆 = ∑(𝐴𝜆𝑖𝑉 + 𝐵𝜆𝑖)𝑒−𝑅𝜆𝑖𝑉 + 𝜔 𝑖=1 where V is the relative volume, E is the energy per unit initial volume, and 𝐴𝑖, 𝑅𝑖, 𝐴𝜆𝑖, 𝐵𝜆𝑖, 𝑅𝜆𝑖, 𝐶, and 𝜔 are input constants defined above. JWLB input constants for some common explosives as found in Baker and Stiel [1997] are given in the following table. E0 (Mbar) DCJ (cm/μs) PCJ (Mbar) A1 (Mbar) A2 (Mbar) A3 (Mbar) A4 (Mbar) R1 R2 R3 R4 C (Mbar) ω Aλ1 Bλ1 Rλ1 Aλ2 Bλ2 Rλ2 TATB 1.800 .07040 .76794 .23740 550.06 22.051 .42788 .28094 16.688 6.8050 2.0737 2.9754 .00776 .27952 1423.9 14387. 19.780 5.0364 -2.6332 1.7062 LX-14 1.821 .10205 .86619 .31717 549.60 64.066 2.0972 .88940 34.636 8.2176 20.401 2.0616 .01251 .38375 18307. 1390.1 19.309 4.4882 -2.6181 1.5076 PETN 1.765 .10910 .83041 .29076 521.96 71.104 4.4774 .97725 44.169 8.7877 25.072 2.2251 .01570 .32357 12.257 52.404 43.932 8.6351 -4.9176 2.1303 *EOS_JWLB Octol 70/30 1.803 .09590 .82994 .29369 526.83 60.579 .91248 .00159 52.106 8.3998 2.1339 .18592 .00968 .39023 .011929 18466. 20.029 5.4192 -3.2394 1.5868 TNT 1.631 .06656 .67174 .18503 490.07 56.868 .82426 .00093 40.713 9.6754 2.4350 .15564 .00710 .30270 .00000 1098.0 15.614 11.468 -6.5011 2.1593 *EOS This is Equation of state Form 15. This EOS works with solid elements and the thick shell using selective reduced 2 × 2 integration (ELFORM = 2 on SECTION_TSHELL) to model the response of gaskets. For the thick shell only, it is completely decoupled from the shell material, i.e., in the local coordinate system of the shell, this model defines the normal stress, 𝜎𝑧𝑧, and does not change any of the other stress components. The model is a reduction of the *MAT_GENERAL_NONLINEAR_6DOF_DISCRETE_BEAM. Card 1 1 2 3 4 5 6 7 8 Variable EOSID LCID1 LCID2 LCID3 LCID4 Type A8 Card 2 1 Variable UNLOAD Type F I 2 K F I 3 I 4 I 5 6 7 8 DMPF TFS CFS LOFFSET IVS F F F F F VARIABLE DESCRIPTION EOSID LCID1 LCID2 LCID3 LCID4 Equation of state ID, a unique number or label not exceeding 8 characters must be specified. Load curve for loading. Load curve for unloading. Load curve for damping as a function of volumetric strain rate. Load curve for scaling the damping as a function of the volumetric strain. *EOS Unload = 0 Loading-unloading curve Unload = 2 Unloading curve *EOS_GASKET Unloading curve ρ∕ρ μ = 0 − 1 Unload = 1 Unload = 3 ρ∕ρ μ = 0 − 1 ρ∕ρ μ = 0 − 1 umin × OFFSET umin Quadratic unloading ρ∕ρ μ = 0 − 1 Figure EOS15-1. Load and unloading behavior. VARIABLE DESCRIPTION UNLOAD Unloading option : EQ.0.0: Loading and unloading follow loading curve EQ.1.0: Loading follows loading curve, unloading follows unloading curve. The unloading curve ID if undefined is taken as the loading curve. EQ.2.0: Loading follows loading curve, unloading follows unloading stiffness, K, to the unloading curve. The loading and unloading curves may only intersect at the origin of the axes. EQ.3.0: Quadratic unloading from peak displacement value to DESCRIPTION a permanent offset. K Unloading stiffness, for UNLOAD = 2 only. *EOS DMPF TFS CFS OFFSET Damping factor for stability. Values in the neighborhood of unity are recommended. The damping factor is properly scaled to eliminate time step size dependency. Tensile failure strain. Compressive failure strain. Offset factor between 0 and 1.0 to determine permanent set upon The permanent sets in unloading if the UNLOAD = 3.0. compression and tension are equal to the product of this offset value and the maximum compressive and tensile displacements, respectively. IVS Initial volume strain. *EOS_MIE_GRUNEISEN This is Equation of state Form 16, a Mie-Gruneisen form with a 𝑝 − 𝛼 compaction model. Card 1 1 2 Variable EOSID GAMMA Type A8 F 3 A1 F 4 A2 F 5 A3 F 6 7 PEL PCO F F 8 N F Default none none none none none none none none 4 5 6 7 8 Card 2 1 Variable ALPHA0 Type F 2 E0 F 3 V0 F Default none none none VARIABLE EOSID DESCRIPTION Equation of state identification. A unique number or label not exceeding 8 characters must be specified. GAMMA Gruneisen gamma. Ai PEL PCO N Hugoniot polynomial coefficient Crush pressure Compaction pressure Porosity exponent ALPHA0 Initial porosity E0 V0 Initial internal energy Initial relative volume *EOS The equation of state is a Mie-Gruneisen form with a polynomial Hugoniot curve and a 𝑝 − 𝛼 compaction model. First, we define a history variable representing the porosity 𝛼 that is initialised to 𝛼0 > 1. The evolution of this variable is given as 𝛼(𝑡) = max ⎜⎛1 + (𝛼0 − 1) [ ⎝ where 𝑝(𝑡) indicates the pressure at time t. For later use, we define the cap pressure as ⎡𝛼0, min𝑠≤𝑡 ⎢ ⎣ 1, min ⎟⎞ ⎠ 𝑝comp − 𝑝(𝑠) ] 𝑝comp − 𝑝𝑒𝑙 }⎫ ⎤ ⎥ ⎭}⎬ ⎦ {⎧ ⎩{⎨ 𝑝𝑐 = 𝑝comp − (𝑝comp − 𝑝𝑒𝑙) [ 1/𝑁 𝛼 − 1 𝛼0 − 1 ] The remainder of the EOS model is given by the equations together with 𝑝(𝜌, 𝑒) = Γ𝛼𝜌𝑒 + 𝑝𝐻(𝜂) [1 − Γ𝜂] 𝑝𝐻(𝜂) = 𝐴1𝜂 + 𝐴2𝜂2 + 𝐴3𝜂3 𝜂(𝜌) = 𝛼𝜌 𝛼0𝜌0 − 1. *EOS_GRUNEISEN This is Equation of state Form 19. This EOS works with SPH elements to model the response of fluids. Card 1 1 2 Variable EOSID GAMMA Type A8 F 3 K0 F 4 V0 F 5 6 7 8 VARIABLE EOSID DESCRIPTION Equation of state ID, a unique number or label not exceeding 8 characters must be specified. GAMMA, K0 Constants in the equation of state. V0 Initial relative volume. Remarks: The Murnaghan equation of state defines pressure as 𝑝 = 𝑘0 [( 𝜌0 ) − 1]. *EOS These are equations of state 21-30. The user can supply his own subroutines. See also Appendix B. The keyword input has to be used for the user interface with data. Card 1 1 2 3 4 5 Variable EOSID EOST LMC NHV IVECT Type A8 I I I I Define LMC material parameters using 8 parameters per card. Card 2 Variable 1 P1 Type F 2 P2 F 3 P3 F 4 P4 F 5 P5 F 6 EO F 6 P6 F 7 VO F 7 P7 F 8 BULK F 8 P8 F VARIABLE EOSID EOST LMC DESCRIPTION Equation of state ID, a unique number or label not exceeding 8 characters must be specified. User equation of state type (21-30 inclusive). A number between 21 and 30 has to be chosen. Length of material constant array which is equal to the number of material constants to be input. (LMC ≤ 48) NHV Number of history variables to be stored, see Appendix B. IVECT EO V0 BULK Vectorization flag (on = 1). A vectorized user subroutine must be supplied. Initial internal energy. Initial relative volume. Bulk modulus. This value is used in the calculation of the contact surface stiffness. Pi Material parameters 𝑖 = 1, … ,LMC. *MAT LS-DYNA has historically referenced each material model by a number. As shown below, a three digit numerical designation can still be used, e.g., *MAT_001, and is equivalent to a corresponding descriptive designation, e.g., *MAT_ELASTIC. The two equivalent commands for each material model, one numerical and the other descriptive, are listed below. The numbers in square brackets identify the element formulations for which the material model is implemented. The number in the curly brackets, {n}, indicates the default number of history variables per element integration point that are stored in addition to the 7 history variables which are stored by default. Just as an example, for the type 16 fully integrated shell elements with 2 integration points through the thickness, the total number of history variables is 8 × (𝑛 + 7). For the Belytschko-Tsay type 2 element the number is 2 × (𝑛 + 7). The meaning associated with particular extra history variables for a subset of material models and equations of state are tabulated at http://www.dynasupport.com/howtos- /material/history-variables. An additional option TITLE may be appended to a *MAT keyword in which case an additional line is read in 80a format which can be used to describe the material. At present, LS-DYNA does not make use of the title. Inclusion of titles simply gives greater clarity to input decks. Key to numbers in square brackets 0 13,14,15) 1H 1B 1I 1T 1D 1SW 2 3a 3c 4 5 6 7 8A - - - - - - - - - - - - - - - Solids (and 2D continuum elements, i.e., shell formulations Hughes-Liu beam Belytschko resultant beam Belytschko integrated solid and tubular beams Truss Discrete beam Spotweld beam Shells Thick shell formulations 1,2,6 Thick shell formulations 3,5,7 Special airbag element SPH element Acoustic solid Cohesive solid Multi-material ALE solid (validated) 8B 9 - - Multi-material ALE solid (implemented but not validated1) Membrane element *MAT_ADD_COHESIVE2 [7] {see associated material model} *MAT_ADD_EROSION2 *MAT_ADD_FATIGUE *MAT_ADD_GENERALIZED_DAMAGE2 [2] *MAT_ADD_PERMEABILTY *MAT_ADD_PORE_AIR *MAT_ADD_THERMAL_EXPANSION2 *MAT_NONLOCAL2 *MAT_ELASTIC [0,1H,1B,1I,1T,2,3a,3c,5,8A] {0} *MAT_{OPTION}TROPIC_ELASTIC [0,2,3a,3c] {15} *MAT_PLASTIC_KINEMATIC [0,1H,1I,1T,2,3a,3c,5,8A] {5} *MAT_ELASTIC_PLASTIC_THERMAL [0,1H,1T,2,3a,3c,5,8B] {3} *MAT_SOIL_AND_FOAM [0,5,3c,8A] {0} *MAT_VISCOELASTIC [0,1H,2,3a,3c,5,8B] {19} *MAT_BLATZ-KO_RUBBER [0,2,3ac,8B] {9} *MAT_HIGH_EXPLOSIVE_BURN [0,5,3c,8A] {4} *MAT_NULL [0,1,2,3c,5,8A] {3} *MAT_ELASTIC_PLASTIC_HYDRO_{OPTION} [0,3c,5,8B] {4} *MAT_STEINBERG [0,3c,5,8B] {5} *MAT_001: *MAT_001_FLUID: *MAT_ELASTIC_FLUID [0,8A] {0} *MAT_002: *MAT_003: *MAT_004: *MAT_005: *MAT_006: *MAT_007: *MAT_008: *MAT_009: *MAT_010: *MAT_011: *MAT_011_LUND: *MAT_STEINBERG_LUND [0,3c,5,8B] {5} *MAT_012: *MAT_013: *MAT_014: *MAT_015: *MAT_016: *MAT_017: *MAT_018: *MAT_019: *MAT_020: *MAT_021: *MAT_022: *MAT_023: *MAT_024: *MAT_025: *MAT_026: *MAT_027: *MAT_028: *MAT_029: *MAT_030: *MAT_ISOTROPIC_ELASTIC_PLASTIC [0,2,3a,3c,5,8B] {0} *MAT_ISOTROPIC_ELASTIC_FAILURE [0,3c,5,8B] {1} *MAT_SOIL_AND_FOAM_FAILURE [0,3c,5,8B] {1} *MAT_JOHNSON_COOK [0,2,3a,3c,5,8A] {6} *MAT_PSEUDO_TENSOR [0,3c,5,8B] {6} *MAT_ORIENTED_CRACK [0,3c] {14} *MAT_POWER_LAW_PLASTICITY [0,1H,2,3a,3c,5,8B] {0} *MAT_STRAIN_RATE_DEPENDENT_PLASTICITY [0,2,3a,3c,5,8B] {6} *MAT_RIGID [0,1H,1B,1T,2,3a] {0} *MAT_ORTHOTROPIC_THERMAL [0,2,3ac] {29} *MAT_COMPOSITE_DAMAGE [0,2,3a,3c,5] {12} *MAT_TEMPERATURE_DEPENDENT_ORTHOTROPIC [0,2,3ac] {19} *MAT_PIECEWISE_LINEAR_PLASTICITY [0,1H,2,3a,3c,5,8A] {5} *MAT_GEOLOGIC_CAP_MODEL [0,3c,5] {12} *MAT_HONEYCOMB [0,3c] {20} *MAT_MOONEY-RIVLIN_RUBBER [0,1T,2,3c,8B] {9} *MAT_RESULTANT_PLASTICITY [1B,2] {5} *MAT_FORCE_LIMITED [1B] {30} *MAT_SHAPE_MEMORY [0,1H,2,3ac,5] {23} 1 Error associated with advection inherently leads to state variables that may be inconsistent with nonlinear constitutive routines and thus may lead to nonphysical results, nonconservation of energy, and even numerical instability in some cases. Caution is advised, particularly when using the 2nd tier of material models implemented for ALE multi-material solids (designated by [8B]) which are largely untested as ALE materials. 2 These commands do not, by themselves, define a material model but rather can be used in certain cases to supplement material models *MAT_FRAZER_NASH_RUBBER_MODEL [0,3c,8B] {9} *MAT_031: *MAT_LAMINATED_GLASS [2,3a] {0} *MAT_032: *MAT_BARLAT_ANISOTROPIC_PLASTICITY [0,2,3a,3c] {9} *MAT_033: *MAT_BARLAT_YLD96 [2,3a] {9} *MAT_033_96: *MAT_FABRIC [4] {17} *MAT_034: *MAT_PLASTIC_GREEN-NAGHDI_RATE [0,3c,5,8B] {22} *MAT_035: *MAT_3-PARAMETER_BARLAT [2,3a] {7} *MAT_036: *MAT_TRANSVERSELY_ANISOTROPIC_ELASTIC_PLASTIC [2,3a] {9} *MAT_037: *MAT_BLATZ-KO_FOAM [0,2,3c,8B] {9} *MAT_038: *MAT_FLD_TRANSVERSELY_ANISOTROPIC [2,3a] {6} *MAT_039: *MAT_NONLINEAR_ORTHOTROPIC [0,2,3c] {17} *MAT_040: *MAT_USER_DEFINED_MATERIAL_MODELS [0,1H,1T,1D,2,3a,3c,5,8B] {0} *MAT_041-050: *MAT_BAMMAN [0,2,3a,3c,5,8B] {8} *MAT_051: *MAT_BAMMAN_DAMAGE [0,2,3a,3c,5,8B] {10} *MAT_052: *MAT_CLOSED_CELL_FOAM [0,3c,8B] {0} *MAT_053: *MAT_ENHANCED_COMPOSITE_DAMAGE [0,2,3c] {20} *MAT_054-055: *MAT_LOW_DENSITY_FOAM [0,3c,5,8B] {26} *MAT_057: *MAT_LAMINATED_COMPOSITE_FABRIC [2,3a] {15} *MAT_058: *MAT_COMPOSITE_FAILURE_{OPTION}_MODEL [0,2,3c,5] {22} *MAT_059: *MAT_ELASTIC_WITH_VISCOSITY [0,2,3a,3c,5,8B] {8} *MAT_060: *MAT_ELASTIC_WITH_VISCOSITY_CURVE [0,2,3a,3c,5,8B] {8} *MAT_060C: *MAT_KELVIN-MAXWELL_VISCOELASTIC [0,3c,5,8B] {14} *MAT_061: *MAT_VISCOUS_FOAM [0,3c,8B] {7} *MAT_062: *MAT_CRUSHABLE_FOAM [0,3c,5,8B] {8} *MAT_063: *MAT_RATE_SENSITIVE_POWERLAW_PLASTICITY [0,2,3a,3c,5,8B] {30} *MAT_064: *MAT_MODIFIED_ZERILLI_ARMSTRONG [0,2,3a,3c,5,8B] {6} *MAT_065: *MAT_LINEAR_ELASTIC_DISCRETE_BEAM [1D] {8} *MAT_066: *MAT_NONLINEAR_ELASTIC_DISCRETE_BEAM [1D] {14} *MAT_067: *MAT_NONLINEAR_PLASTIC_DISCRETE_BEAM [1D] {25} *MAT_068: *MAT_SID_DAMPER_DISCRETE_BEAM [1D] {13} *MAT_069: *MAT_HYDRAULIC_GAS_DAMPER_DISCRETE_BEAM [1D] {8} *MAT_070: *MAT_CABLE_DISCRETE_BEAM [1D] {8} *MAT_071: *MAT_CONCRETE_DAMAGE [0,3c,5,8B] {6} *MAT_072: *MAT_CONCRETE_DAMAGE_REL3 [0,3c,5] {6} *MAT_072R3: *MAT_LOW_DENSITY_VISCOUS_FOAM [0,3c,8B] {56} *MAT_073: *MAT_ELASTIC_SPRING_DISCRETE_BEAM [1D] {8} *MAT_074: *MAT_BILKHU/DUBOIS_FOAM [0,3c,5,8B] {8} *MAT_075: *MAT_GENERAL_VISCOELASTIC [0,2,3a,3c,5,8B] {53} *MAT_076: *MAT_HYPERELASTIC_RUBBER [0,2,3c,5,8B] {54} *MAT_077_H: *MAT_OGDEN_RUBBER [0,2,3c,8B] {54} *MAT_077_O: *MAT_SOIL_CONCRETE [0,3c,5,8B] {3} *MAT_078: *MAT_HYSTERETIC_SOIL [0,3c,5,8B] {96} *MAT_079: *MAT_RAMBERG-OSGOOD [0,3c,8B] {18} *MAT_080: *MAT_081: *MAT_PLASTICITY_WITH_DAMAGE [0,2,3a,3c] {5} *MAT_082(_RCDC): *MAT_PLASTICITY_WITH_DAMAGE_ORTHO(_RCDC) [0,2,3a,3c] {22} *MAT_083: *MAT_084: *MAT_086: *MAT_087: *MAT_088: *MAT_089: *MAT_090: *MAT_091: *MAT_092: *MAT_FU_CHANG_FOAM [0,3c,5,8B] {54} *MAT_WINFRITH_CONCRETE [0] {54} *MAT_ORTHOTROPIC_VISCOELASTIC [2,3a] {17} *MAT_CELLULAR_RUBBER [0,3c,5,8B] {19} *MAT_MTS [0,2,3a,3c,5,8B] {5} *MAT_PLASTICITY_POLYMER [0,2,3a,3c] {46} *MAT_ACOUSTIC [6] {25} *MAT_SOFT_TISSUE [0,2] {16} *MAT_SOFT_TISSUE_VISCO [0,2] {58} *MAT_094: *MAT_095: *MAT_096: *MAT_097: *MAT_098: *MAT_099: {22} *EOS_USER_DEFINED *MAT_ELASTIC_6DOF_SPRING_DISCRETE_BEAM [1D] {25} *MAT_INELASTIC_SPRING_DISCRETE_BEAM [1D] {9} *MAT_INELASTIC_6DOF_SPRING_DISCRETE_BEAM [1D] {25} *MAT_BRITTLE_DAMAGE [0,8B] {51} *MAT_GENERAL_JOINT_DISCRETE_BEAM [1D] {23} *MAT_SIMPLIFIED_JOHNSON_COOK [0,1H,1B,1T,2,3a,3c] {6} *MAT_SIMPLIFIED_JOHNSON_COOK_ORTHOTROPIC_DAMAGE [0,2,3a,3c] *MAT_100: *MAT_100_DA: *MAT_101: *MAT_102(_T): *MAT_103: *MAT_103_P: *MAT_104: *MAT_105: *MAT_106: *MAT_107: *MAT_108: *MAT_110: *MAT_111: *MAT_112: *MAT_113: *MAT_114: *MAT_115: *MAT_115_O: *MAT_116: *MAT_117: *MAT_118: *MAT_119: *MAT_120: *MAT_120_JC: *MAT_120_RCDC: *MAT_121: *MAT_122: *MAT_122_3D: *MAT_123: *MAT_124: *MAT_125: *MAT_126: *MAT_127: *MAT_128: *MAT_129: *MAT_130: *MAT_131: *MAT_132: *MAT_133: *MAT_134: *MAT_135: *MAT_135_PLC: *MAT_136: *MAT_138: *MAT_139: *MAT_140: *MAT_SPOTWELD_{OPTION} [0,1SW] {6} *MAT_SPOTWELD_DAIMLERCHRYSLER [0] {6} *MAT_GEPLASTIC_SRATE_2000a [2,3a] {15} *MAT_INV_HYPERBOLIC_SIN(_THERMAL) [0,3c,8B] {15} *MAT_ANISOTROPIC_VISCOPLASTIC [0,2,3a,3c,5] {20} *MAT_ANISOTROPIC_PLASTIC [2,3a,3c] {20} *MAT_DAMAGE_1 [0,2,3a,3c] {11} *MAT_DAMAGE_2 [0,2,3a,3c] {7} *MAT_ELASTIC_VISCOPLASTIC_THERMAL [0,2,3a,3c,5] {20} *MAT_MODIFIED_JOHNSON_COOK [0,2,3a,3c,5,8B] {15} *MAT_ORTHO_ELASTIC_PLASTIC [2,3a] {15} *MAT_JOHNSON_HOLMQUIST_CERAMICS [0,3c,5] {15} *MAT_JOHNSON_HOLMQUIST_CONCRETE [0,3c,5] {25} *MAT_FINITE_ELASTIC_STRAIN_PLASTICITY [0,3c,5] {22} *MAT_TRIP [2,3a] {5} *MAT_LAYERED_LINEAR_PLASTICITY [2,3a] {13} *MAT_UNIFIED_CREEP [0,2,3a,3c,5] {1} *MAT_UNIFIED_CREEP_ORTHO [0,3c,5] {1} *MAT_COMPOSITE_LAYUP [2] {30} *MAT_COMPOSITE_MATRIX [2] {30} *MAT_COMPOSITE_DIRECT [2] {10} *MAT_GENERAL_NONLINEAR_6DOF_DISCRETE_BEAM [1D] {62} *MAT_GURSON [0,2,3a,3c] {12} *MAT_GURSON_JC [0,2] {12} *MAT_GURSON_RCDC [0,2] {12} *MAT_GENERAL_NONLINEAR_1DOF_DISCRETE_BEAM [1D] {20} *MAT_HILL_3R [2,3a] {8} *MAT_HILL_3R_3D [0] {28} *MAT_MODIFIED_PIECEWISE_LINEAR_PLASTICITY [0,2,3a,3c,5] {11} *MAT_PLASTICITY_COMPRESSION_TENSION [0,1H,2,3a,3c,5,8B] {7} *MAT_KINEMATIC_HARDENING_TRANSVERSELY_ANISOTROPIC [0,2,3a,3c] {11} *MAT_MODIFIED_HONEYCOMB [0,3c] {20} *MAT_ARRUDA_BOYCE_RUBBER [0,3c,5] {49} *MAT_HEART_TISSUE [0,3c] {15} *MAT_LUNG_TISSUE [0,3c] {49} *MAT_SPECIAL_ORTHOTROPIC [2] {35} *MAT_ISOTROPIC_SMEARED_CRACK [0,5,8B] {15} *MAT_ORTHOTROPIC_SMEARED_CRACK [0] {61} *MAT_BARLAT_YLD2000 [2,3a] {9} *MAT_VISCOELASTIC_FABRIC [9] *MAT_WTM_STM [2,3a] {30} *MAT_WTM_STM_PLC [2,3a] {30} *MAT_CORUS_VEGTER [2,3a] {5} *MAT_COHESIVE_MIXED_MODE [7] {0} *MAT_MODIFIED_FORCE_LIMITED [1B] {35} *MAT_VACUUM [0,8A] {0} *MAT_141: *MAT_142: *MAT_143: *MAT_144: *MAT_145: *MAT_146: *MAT_147 *MAT_147_N: *MAT_148: *MAT_151: *MAT_153: *MAT_154: *MAT_155: *MAT_156: *MAT_157: *MAT_158: *MAT_159: *MAT_160: *MAT_161: *MAT_162: *MAT_163 *MAT_164: *MAT_165: *MAT_165B: *MAT_166: *MAT_167: *MAT_168: *MAT_169: *MAT_170: *MAT_171: *MAT_172: *MAT_173: *MAT_174: *MAT_175: *MAT_176: *MAT_177: *MAT_178: *MAT_179: *MAT_181: *MAT_183: *MAT_184: *MAT_185: *MAT_186: *MAT_187: *MAT_188: *MAT_189: *MAT_190: *MAT_191: *MAT_192: *MAT_193: *MAT_194: *MAT_195: *MAT_196: *MAT_197: *MAT_RATE_SENSITIVE_POLYMER [0,3c,8B] {6} *MAT_TRANSVERSELY_ISOTROPIC_CRUSHABLE_FOAM [0,3c] {12} *MAT_WOOD_{OPTION} [0,3c,5] {37} *MAT_PITZER_CRUSHABLE_FOAM [0,3c,8B] {7} *MAT_SCHWER_MURRAY_CAP_MODEL [0,5] {50} *MAT_1DOF_GENERALIZED_SPRING [1D] {1} *MAT_FHWA_SOIL [0,3c,5,8B] {15} *MAT_FHWA_SOIL_NEBRASKA [0,3c,5,8B] {15} *MAT_GAS_MIXTURE [0,8A] {14} *MAT_EMMI [0,3c,5,8B] {23} *MAT_DAMAGE_3 [0,1H,2,3a,3c] *MAT_DESHPANDE_FLECK_FOAM [0,3c,8B] {10} *MAT_PLASTICITY_COMPRESSION_TENSION_EOS [0,3c,5,8B] {16} *MAT_MUSCLE [1T] {0} *MAT_ANISOTROPIC_ELASTIC_PLASTIC [0,2,3a] {5} *MAT_RATE_SENSITIVE_COMPOSITE_FABRIC [2,3a] {54} *MAT_CSCM_{OPTION} [0,3c,5] {22} *MAT_ALE_INCOMPRESSIBLE *MAT_COMPOSITE_MSC [0] {34} *MAT_COMPOSITE_DMG_MSC [0] {40} *MAT_MODIFIED_CRUSHABLE_FOAM [0,3c,8B] {10} *MAT_BRAIN_LINEAR_VISCOELASTIC [0] {14} *MAT_PLASTIC_NONLINEAR_KINEMATIC [0,2,3a,3c,8B] {8} *MAT_PLASTIC_NONLINEAR_KINEMATIC_B [0,2] *MAT_MOMENT_CURVATURE_BEAM [1B] {54} *MAT_MCCORMICK [03c,,8B] {8} *MAT_POLYMER [0,3c,8B] {60} *MAT_ARUP_ADHESIVE [0] {30} *MAT_RESULTANT_ANISOTROPIC [2,3a] {67} *MAT_STEEL_CONCENTRIC_BRACE [1B] {35} *MAT_CONCRETE_EC2 [1H,2,3a] {64} *MAT_MOHR_COULOMB [0,5] {52} *MAT_RC_BEAM [1H] {22} *MAT_VISCOELASTIC_THERMAL [0,2,3a,3c,5,8B] {86} *MAT_QUASILINEAR_VISCOELASTIC [0,2,3a,3c,5,8B] {81} *MAT_HILL_FOAM [0,3c] {12} *MAT_VISCOELASTIC_HILL_FOAM [0,3c] {92} *MAT_LOW_DENSITY_SYNTHETIC_FOAM_{OPTION} [0,3c] {77} *MAT_SIMPLIFIED_RUBBER/FOAM_{OPTION} [0,2,3c] {39} *MAT_SIMPLIFIED_RUBBER_WITH_DAMAGE [0,2,3c] {44} *MAT_COHESIVE_ELASTIC [7] {0} *MAT_COHESIVE_TH [7] {0} *MAT_COHESIVE_GENERAL [7] {6} *MAT_SAMP-1 [0,2,3a,3c] {38} *MAT_THERMO_ELASTO_VISCOPLASTIC_CREEP [0,2,3a,3c] {27} *MAT_ANISOTROPIC_THERMOELASTIC [0,3c,8B] {21} *MAT_FLD_3-PARAMETER_BARLAT [2,3a] {36} *MAT_SEISMIC_BEAM [1B] {36} *MAT_SOIL_BRICK [0,3c] {96} *MAT_DRUCKER_PRAGER [0,3c] {24} *MAT_RC_SHEAR_WALL [2,3a] {36} *MAT_CONCRETE_BEAM [1H] {5} *MAT_GENERAL_SPRING_DISCRETE_BEAM [1D] {25} *MAT_SEISMIC_ISOLATOR [1D] {20} *MAT_JOINTED_ROCK [0] {31} *MAT_STEEL_EC3 [1H] {3} *MAT_HYSTERETIC_REINFORCEMENT [1H,2] {64} *MAT_BOLT_BEAM [1D] {16} *MAT_SPR_JLR [1H] {60} *MAT_DRY_FABRIC [9] *MAT_4A_MICROMEC [0,2,3a,3c] *MAT_ELASTIC_PHASE_CHANGE [0] *MAT_OPTION_TROPIC_ELASTIC_PHASE_CHANGE [0] *MAT_MOONEY-RIVLIN_RUBBER_PHASE_CHANGE [0] *MAT_CODAM2 [0,2,3a,3c] *MAT_RIGID_DISCRETE [0,2] *MAT_ORTHOTROPIC_SIMPLIFIED_DAMAGE [0,3c,5] {17} *MAT_TABULATED_JOHNSON_COOK [0,2,3a,3c,,5] {17} *MAT_TABULATED_JOHNSON_COOK_GYS [0] {17} *MAT_VISCOPLASTIC_MIXED_HARDENING [0,2,3a,3c,5] *MAT_KINEMATIC_HARDENING_BARLAT89 [2,3a] *MAT_PML_ELASTIC [0] {24} *MAT_PML_ACOUSTIC [6] {35} *MAT_BIOT_HYSTERETIC [0,2,3a] {30} *MAT_CAZACU_BARLAT [2,3a] *MAT_VISCOELASTIC_LOOSE_FABRIC [2,3a] *MAT_MICROMECHANICS_DRY_FABRIC [2,3a] *MAT_SCC_ON_RCC [2,3a] *MAT_PML_HYSTERETIC [0] {54} *MAT_PERT_PIECEWISE_LINEAR_PLASTICITY [0,1H,2,3,5,8A] *MAT_COHESIVE_MIXED_MODE_ELASTOPLASTIC_RATE [7] {0} *MAT_JOHNSON_HOLMQUIST_JH1 [0,3c,5] *MAT_KINEMATIC_HARDENING_BARLAT2000 [2,3a] *MAT_HILL_90 [2,3a] *MAT_UHS_STEEL [0,2,3a,3c,5] {35} *MAT_PML_{OPTION}TROPIC_ELASTIC [0] {30} *MAT_PML_NULL [0] {27} *MAT_PHS_BMW [2] {38} *MAT_REINFORCED_THERMOPLASTIC [2] *MAT_198: *MAT_202: *MAT_203: *MAT_208: *MAT_211: *MAT_214: *MAT_215: *MAT_216: *MAT_217: *MAT_218: *MAT_219: *MAT_220: *MAT_221: *MAT_224: *MAT_224_GYS: *MAT_225: *MAT_226: *MAT_230: *MAT_231: *MAT_232: *MAT_233: *MAT_234: *MAT_235: *MAT_236: *MAT_237: *MAT_238: *MAT_240: *MAT_241: *MAT_242: *MAT_243: *MAT_244: *MAT_245: *MAT_246: *MAT_248: *MAT_249: *MAT_249_UDFIBER: *MAT_REINFORCED_THERMOPLASTIC_UDFIBER [2] *MAT_251: *MAT_252: *MAT_254: *MAT_255: *MAT_256: *MAT_260A: *MAT_260B: *MAT_261: *MAT_262: *MAT_264: *MAT_266: *MAT_267: *MAT_269: *MAT_270: *MAT_271: *MAT_272: *MAT_273: *MAT_274: *MAT_TAILORED_PROPERTIES [2] {6} *MAT_TOUGHENED_ADHESIVE_POLYMER [0,7] {10} *MAT_GENERALIZED_PHASE_CHANGE [0,2] *MAT_PIECEWISE_LINEAR_PLASTIC_THERMAL [0,2,3a,3c] *MAT_AMORPHOUS_SOLIDS_FINITE_STRAIN [0] *MAT_STOUGHTON_NON_ASSOCIATED_FLOW [0,2] *MAT_MOHR_NON_ASSOCIATED_FLOW [0,2] *MAT_LAMINATED_FRACTURE_DAIMLER_PINHO [0,2,3a,3c] *MAT_LAMINATED_FRACTURE_DAIMLER_CAMANHO [0,2,3a,3c] *MAT_TABULATED_JOHNSON_COOK_ORTHO_PLASTICITY [0] *MAT_TISSUE_DISPERSED [0] *MAT_EIGHT_CHAIN_RUBBER [0,5] *MAT_BERGSTROM_BOYCE_RUBBER [0,5] *MAT_CWM [0,2,5] *MAT_POWDER [0,5] *MAT_RHT [0,5] *MAT_CONCRETE_DAMAGE_PLASTIC_MODEL [0] *MAT_PAPER [0,2] *MAT_275: *MAT_276: *MAT_277: *MAT_278: *MAT_279: *MAT_280: *MAT_293: *MAT_SMOOTH_VISCOELASTIC_VISCOPLASTIC [0] *MAT_CHRONOLOGICAL_VISCOELASTIC [2,3a,3c] *MAT_ADHESIVE_CURING_VISCOELASTIC [0] *MAT_CF_MICROMECHANICS [02] {3} *MAT_COHESIVE_PAPER [7] *MAT_GLASS [2] {32} *MAT_COMPRF [2] {7} For the discrete (type 6) beam elements, which are used to model complicated dampers and multi-dimensional spring-damper combinations, the following material types are available: *MAT_066: *MAT_067: *MAT_068: *MAT_069: *MAT_070: *MAT_071: *MAT_074: *MAT_093: *MAT_094: *MAT_095: *MAT_119: *MAT_121: *MAT_146: *MAT_196: *MAT_197: *MAT_208: *MAT_LINEAR_ELASTIC_DISCRETE_BEAM [1D] *MAT_NONLINEAR_ELASTIC_DISCRETE_BEAM [1D] *MAT_NONLINEAR_PLASTIC_DISCRETE_BEAM [1D] *MAT_SID_DAMPER_DISCRETE_BEAM [1D] *MAT_HYDRAULIC_GAS_DAMPER_DISCRETE_BEAM [1D] *MAT_CABLE_DISCRETE_BEAM [1D] *MAT_ELASTIC_SPRING_DISCRETE_BEAM [1D] *MAT_ELASTIC_6DOF_SPRING_DISCRETE_BEAM [1D] *MAT_INELASTIC_SPRING_DISCRETE_BEAM [1D] *MAT_INELASTIC_6DOF_SPRING_DISCRETE_BEAM [1D] *MAT_GENERAL_NONLINEAR_6DOF_DISCRETE_BEAM [1D] *MAT_GENERAL_NONLINEAR_1DOF_DISCRETE_BEAM [1D] *MAT_1DOF_GENERALIZED_SPRING [1D] *MAT_GENERAL_SPRING_DISCRETE_BEAM [1D] *MAT_SEISMIC_ISOLATOR [1D] *MAT_BOLT_BEAM [1D] For the discrete springs and dampers the following material types are available *MAT_S01: *MAT_S02: *MAT_S03: *MAT_S04: *MAT_S05: *MAT_S06: *MAT_S07: *MAT_S08: *MAT_S13: *MAT_S14: *MAT_S15: *MAT_SPRING_ELASTIC *MAT_DAMPER_VISCOUS *MAT_SPRING_ELASTOPLASTIC *MAT_SPRING_NONLINEAR_ELASTIC *MAT_DAMPER_NONLINEAR_VISCOUS *MAT_SPRING_GENERAL_NONLINEAR *MAT_SPRING_MAXWELL *MAT_SPRING_INELASTIC *MAT_SPRING_TRILINEAR_DEGRADING *MAT_SPRING_SQUAT_SHEARWALL *MAT_SPRING_MUSCLE For ALE solids the following material types are available: *MAT_ALE_01: *MAT_ALE_02: *MAT_ALE_03: *MAT_ALE_04: *MAT_ALE_05: *MAT_ALE_06: *MAT_ALE_VACUUM *MAT_ALE_GAS_MIXTURE *MAT_ALE_VISCOUS *MAT_ALE_MIXING_LENGTH *MAT_ALE_INCOMPRESSIBLE *MAT_ALE_HERSCHEL (same as *MAT_140) (same as *MAT_148) (same as *MAT_009) (same as *MAT_149) (same as *MAT_160) For SPH particles the following material type is available: *MAT_SPH_01: *MAT_SPH_VISCOUS (same as *MAT_009) For the seatbelts one material is available. *MAT_B01: *MAT_SEATBELT For thermal materials in a coupled structural/thermal or thermal only analysis, six materials are available. These materials are related to the structural material via the *PART card. *MAT_T01: *MAT_T02: *MAT_T03: *MAT_T04: *MAT_T05: *MAT_T07: *MAT_T08 *MAT_T09 *MAT_T10 *MAT_T11-T15: *MAT_THERMAL_ISOTROPIC *MAT_THERMAL_ORTHOTROPIC *MAT_THERMAL_ISOTROPIC_TD *MAT_THERMAL_ORTHOTROPIC_TD *MAT_THERMAL_DISCRETE_BEAM *MAT_THERMAL_CWM *MAT_THERMAL_ORTHOTROPIC_TD_LC *MAT_THERMAL_ISOTROPIC_PHASE_CHANGE *MAT_THERMAL_ISOTROPIC_TD_LC *MAT_THERMAL_USER_DEFINED DEFINED Remarks: Curves and tables are sometimes defined for the purpose of defining material properties. An example would be a curve of effective stress vs. effective plastic strain defined using the command *DEFINE_CURVE. In general, the following can be said about curves and tables that are referenced by material models: 1. Curves are internally rediscretized using equal increments along the 𝑥-axis. 2. Curve data is interpolated between rediscretized data points within the defined range of the curve and extrapolated as needed beyond the defined range of the curve. 3. Extrapolation is not employed for table values see the manual entries for the *DEFINE_TABLE_… keywords. MATERIAL MODEL REFERENCE TABLES The tables provided on the following pages list the material models, some of their attributes, and the general classes of physical materials to which the numerical models might be applied. If a material model, without consideration of *MAT_ADD_EROSION, *MAT_ADD_- THERMAL_EXPANSION, or *MAT_ADD_GENERALIZED_DAMAGE, includes any of the following attributes, a “Y” will appear in the respective column of the table: SRATE FAIL EOS - Strain-rate effects - Failure criteria - Equation-of-State required for 3D solids and 2D continuum elements THERMAL - Thermal effects ANISO DAM TENS - Anisotropic/orthotropic - Damage effects - Tension handled differently than compression in some manner Potential applications of the material models, in terms of classes of physical materials, are abbreviated in the table as follows: GN - General CM - Composite CR - Ceramic FL - Fluid FM - Foam GL - Glass HY - Hydrodynamic material MT - Metal - Plastic PL RB - Rubber SL AD - Adhesive or Cohesive material BIO - Biological material CIV - Civil Engineering component HT - Heat Transfer F - Soil, concrete, or rock - Fabric Y Y Material Number And Description Elastic Orthotropic Elastic (Anisotropic-solids) Plastic Kinematic/Isotropic Y Y Elastic Plastic Thermal Soil and Foam Linear Viscoelastic Blatz-Ko Rubber High Explosive Burn Null Material Y Y Y Y Y Elastic Plastic Hydro(dynamic) Y Y APPS GN, FL CM, MT CM, MT, PL MT, PL Y FM, SL RB RB HY FL, HY HY, MT HY, MT MT Y Y Y Steinberg: Temp. Dependent Elastoplastic Isotropic Elastic Plastic Isotropic Elastic with Failure Soil and Foam with Failure Y Y Y Y Y Y Y MT Y FM, SL Johnson/Cook Plasticity Model Y Y Y Y Y Y Pseudo Tensor Geological Model Y Y Y Y Y Oriented Crack (Elastoplastic w/ Fracture) Y Y Y Y Power Law Plasticity (Isotropic) Y Strain Rate Dependent Plasticity Y Y Rigid Orthotropic Thermal (Elastic) Y Y HY, MT SL HY, MT, PL, CR MT, PL MT, PL GN 2-10 (EOS) LS-DYNA R10.0 1 2 3 4 5 6 7 8 9 10 11 12 13 14 15 16 17 18 19 Material Number And Description Composite Damage Y Y Temperature Dependent Orthotropic Y Y Piecewise Linear Plasticity (Isotropic) Y Y Inviscid Two Invariant Geologic Cap Y Honeycomb Y Y Y Mooney-Rivlin Rubber Resultant Plasticity Force Limited Resultant Formulation Shape Memory Frazer-Nash Rubber Laminated Glass (Composite) Y Barlat Anisotropic Plasticity (YLD96) Fabric Plastic-Green Naghdi Rate Three-Parameter Barlat Plasticity Transversely Anisotropic Elastic Plastic Y Y Y Y Y Y Y Y Y Blatz-Ko Foam FLD Transversely Anisotropic Nonlinear Orthotropic -50 User Defined Materials Y Y Y Y Y Y Y Y Y Y Y Bamman (Temp/Rate Dependent Plasticity) Bamman Damage Closed cell foam (Low density polyurethane) Composite Damage with Chang Failure Composite Damage with Tsai-Wu Failure Low Density Urethane Foam Laminated Composite Fabric Y Y Y Y Y Y Y Y Y Y Y Y Y Y Y Y Y Y LS-DYNA R10.0 Y Y Y CM, F 2-11 (EOS) Y Y Y Y Y Y APPS CM CM MT, PL SL CM, FM, SL RB MT MT RB CM, GL CR, MT Y F MT MT MT FM, PL MT CM GN GN MT FM CM CM FM 22 23 24 25 26 27 28 29 30 31 32 33 34 35 36 37 38 39 40 41 51 52 53 54 55 Material Number And Description Composite Failure (Plasticity Based) Elastic with Viscosity (Viscous Glass) Kelvin-Maxwell Viscoelastic Viscous Foam (Crash dummy Foam) Isotropic Crushable Foam Rate Sensitive Powerlaw Plasticity Y Y Y Y Y Y Y Y Y APPS CM, CR GL FM FM FM MT Zerilli-Armstrong (Rate/Temp Plasticity) Y Y Y Y MT Linear Elastic Discrete Beam Nonlinear Elastic Discrete Beam Y Y Nonlinear Plastic Discrete Beam Y Y SID Damper Discrete Beam Hydraulic Gas Damper Discrete Beam Cable Discrete Beam (Elastic) Y Y Y Y Y Y Y Cables Concrete Damage (incl. Release III) Y Y Y Y Y Low Density Viscous Foam Elastic Spring Discrete Beam Bilkhu/Dubois Foam General Viscoelastic (Maxwell Model) Hyperelastic and Ogden Rubber Soil Concrete Hysteretic Soil (Elasto-Perfectly Plastic) Ramberg-Osgood Plasticity with Damage Plasticity with Damage Ortho Fu Chang Foam Winfrith Concrete Orthotropic Viscoelastic Cellular Rubber MTS Plasticity Polymer Y Y Y Y Y Y Y Y Y Y Y Y Y Y Y Y Y Y Y SL FM FM RB RB SL SL SL MT, PL Y Y Y Y Y Y Y Y Y Y Y Y Y Y Y Y Y FM Y FM, SL RB RB MT PL Y Y LS-DYNA R10.0 59 60 61 62 63 64 65 66 67 68 69 70 71 72 73 74 75 76 77 78 79 80 81 82 83 84 86 87 88 Material Number And Description 90 91 92 93 94 95 96 97 98 99 100 101 Acoustic Soft Tissue Soft Tissue (viscous) Elastic 6DOF Spring Discrete Beam Inelastic Spring Discrete Beam Inelastic 6DOF Spring Discrete Beam Brittle Damage General Joint Discrete Beam Simplified Johnson Cook Simpl. Johnson Cook Orthotropic Damage Spotweld GE Plastic Strain Rate Y Y Y Y Y Y Y Y Y Y Y Y Y Y Y Y Y Y 102(_T) Inv. Hyperbolic Sin (Thermal) Y Y 103 103P Anisotropic Viscoplastic Anisotropic Plastic Y Y Y Y Y Y Y Y Y Y Y Y Y Y Y Y Y Damage 1 Damage 2 Elastic Viscoplastic Thermal Modified Johnson Cook Ortho Elastic Plastic Johnson Holmquist Ceramics Johnson Holmquist Concrete Finite Elastic Strain Plasticity 104 105 106 107 108 110 111 112 113 114 115 115_O 116 Unified Creep Unified Creep Ortho Composite Layup Transformation Induced Plasticity (TRIP) Layered Linear Plasticity Y Y APPS FL BIO Y Y Y Y Y Y Y Y Y Y Y SL Y Y MT MT Y Y MT Y Y Y Y Y Y Y Y Y Y Y Y Y Y PL MT, PL MT MT MT MT PL MT CR, GL SL PL MT MT, PL, CM GN GN CM Material Number And Description 117 118 119 120 121 122 Composite Matrix Composite Direct General Nonlinear 6DOF Discrete Beam Gurson General Nonlinear 1DOF Discrete Beam Hill 3RC 122_3D Hill 3R 3D Modified Piecewise Linear Plasticity Plasticity Compression Tension Kinematic Hardening Transversely Aniso. Y Y Y Y Y Y Y Y Y Y Y Y Y Y Y Y 123 124 125 126 127 128 129 130 131 132 133 134 135 136 138 139 140 141 142 143 Modified Honeycomb Y Y Y Y Y Arruda Boyce Rubber Heart Tissue Lung Tissue Special Orthotropic Isotropic Smeared Crack Orthotropic Smeared Crack Barlat YLD2000 Viscoelastic Fabric Y Y Y Y Y Y Y Y Y Y Y Y Y Y Y Weak and Strong Texture Model Y Y Corus Vegter Cohesive Mixed Mode Modified Force Limited Vacuum Y Y Y Y Y Y Y Y Rate Sensitive Polymer Y Transversely Isotropic Crushable Foam PL FM Y Wood Y Y Y Y Y Wood 2-14 (EOS) LS-DYNA R10.0 APPS CM CM Y Y Y MT Y Y MT MT, CM MT, PL MT, PL MT CM, FM, SL RB BIO BIO MT, CM MT, CM MT MT Y Y Y Y Y Y Y Y Y Y Y Y Y Y Y Y Y Y Y Material Number And Description 144 145 146 147 Pitzer Crushable Foam Schwer Murray Cap Model 1DOF Generalized Spring FWHA Soil 147N FHWA Soil Nebraska Gas Mixture Evolving Microstructural Model of Inelast. 148 151 153 154 155 156 157 158 159 160 Damage 3 Deshpande Fleck Foam Y Y Y Plasticity Compression Tension EOS Y Y Y Muscle Anisotropic Elastic Plastic Rate-Sensitive Composite Fabric CSCM ALE incompressible Y Y Y Y Y Y Y Y Y Y Y Y Y Y 161,162 Composite MSC (Dmg) Y Y Y Y Y 163 164 165 165B 166 167 168 169 170 171 172 173 174 Modified Crushable Foam Brain Linear Viscoelastic Plastic Nonlinear Kinematic Plastic Nonlinear Kinematic_B Moment Curvature Beam McCormick Polymer Arup Adhesive Resultant Anisotropic Steel Concentric Brace Concrete EC2 Mohr Coulomb RC Beam Y Y Y Y Y Y Y Y Y Y Y Y Y Y Y Y Y Y Y Y Y Y Y Y APPS FM SL SL SL FL MT MT, PL FM Ice BIO MT, CM CM SL CM FM BIO MT MT CIV MT PL AD PL CIV SL, MT SL SL Y Y Material Number And Description Viscoelastic Thermal Quasilinear Viscoelastic Hill Foam Viscoelastic Hill Foam (Ortho) Low Density Synthetic Foam Simplified Rubber/Foam Simplified Rubber with Damage Cohesive Elastic Cohesive TH Cohesive General Semi-Analytical Model for Polymers – 1 Thermo Elasto Viscoelastic Creep Anisotropic Thermoelastic Y Y Y Y Y Y Y Y Y Y Y Y Y Y Y Y Y Y Y Y Y Y Y Y Y Y Y Y Y Y Y Y Y Y Y APPS RB BIO FM FM FM RB, FM RB AD AD AD PL MT Y Y Y Flow limit diagram 3-Parameter Barlat Y Seismic Beam Soil Brick Drucker Prager RC Shear Wall Concrete Beam General Spring Discrete Beam Seismic Isolator Jointed Rock Steel EC3 Hysteretic Reinforcement Bolt Beam SPR JLR Dry Fabric 4A Micromec Elastic Phase Change Orthotropic Elastic Phase Change Mooney Rivlin Rubber Phase Change Y Y Y Y Y Y Y Y Y Y Y Y Y Y Y Y Y Y Y Y MT Y CIV Y Y Y Y Y Y Y Y Y Y SL SL CIV CIV CIV SL CIV CV Y Y MT MT Y Y Y Y Y CM,PL Y GN GN RB Y LS-DYNA R10.0 175 176 177 178 179 181 183 184 185 186 187 188 189 190 191 192 193 194 195 196 197 198 202 203 208 211 214 215 216 217 Material Number And Description CODAM2 Rigid Discrete Orthotropic Simplified Damage Y Y APPS Y Y Y CM Y Y Y Tabulated Johnson Cook Y Y Y Y Y Y 219 220 221 224 224_GYS Tabulated Johnson Cook GYS Y Y Y Y Y Y 225 226 230 231 232 233 234 235 236 237 238 240 241 242 243 244 245 246 248 249 Viscoplastic Mixed Hardening Y Y Kinematic hardening Barlat 89 Elastic Perfectly Matched Layer (PML) Acoustic PML Biot Linear Hysteretic Material Cazacu Barlat Viscoelastic Loose Fabric Micromechanic Dry Fabric Ceramic Matrix Biot Hysteretic PML Piecewise linear plasticity (PERT) Cohesive mixed mode Johnson Holmquist JH1 Kinematic hardening Barlat 2000 Hill 90 UHS Steel Orthotropic/anisotropic PML Null material PML PHS BMW Reinforced Thermoplastic Y Y Y Y Y Y Y Y Y Y Y Y Y Y Y Y LS-DYNA R10.0 Y Y Y Y Y Y Y Y Y Y Y Y Y Y Y Y Y Y Y Y MT Y Y Y CM HY, MT, PL HY, MT, PL MT, PL MT SL FL SL Fabric Fabric CM, CR SL MT, PL AD CR, GL MT MT MT SL FL MT Material Number And Description APPS 249_ UDfiber Reinforced Thermoplastic UDfiber Y Y Y CM, F 251 252 254 255 256 260A 260B 261 262 264 266 267 269 270 271 272 273 274 275 276 277 278 279 280 293 A01 A02 A03 Tailored Properties Y Y Toughened Adhesive Polymer Y Y Y Y Y Y Generalized Phase Change Piecewise linear plastic thermal Amorphous solid (finite strain) Stoughton non-associated flow Y Y Y Y Y Y Y Y MT Y Y Mohr non-associated flow Y Y Y Y Y Laminated Fracture Daimler Pinho Laminated Fracture Daimler Camanho Y Y Y Y Y Y Y Y Tabulated Johnson Cook Orthotorpic Plasticity Y Y Y Y Y Y Y MT, PL AD MT GL MT MT CM CM HY, MT, PL BIO Dispersed tissue Eight chain rubber Bergström Boyce rubber Welding material Powder compaction RHT concrete model Concrete damage plastic Paper Smooth viscoelastic viscoplastic Chronological viscoelastic Adhesive curing viscoelastic CF Micromechanics Cohesive Paper Glass COMPRF ALE Vacuum ALE Gas Mixture ALE Viscous Y Y Y Y Y Y Y Y Y Y Y Y Y Y Y RB, PL RB MT,PL Y CR,SL Y Y SL,CIV Y Y SL Y CM,PL MT,PL RB PL,RB Y Y Y Y Y Y Y Y Y Y Y Y Y Y Y CM AD GL CM FL FL FL APPS Material Number And Description A04 A05 A06 ALE Mixing Length ALE Incompressible ALE Herschel SPH01 SPH Viscous S1 S2 S3 S4 S5 S6 S7 S8 S13 S14 S15 B1 T01 T02 T03 T04 T05 T07 T08 T09 T10 T11 Y Y Y Y Y Spring Elastic (Linear) Damper Viscous (Linear) Spring Elastoplastic (Isotropic) Spring Nonlinear Elastic Damper Nonlinear Viscous Spring General Nonlinear Spring Maxwell (3-Parameter Viscoelastic) Spring Inelastic (Tension or Compression) Spring Trilinear Degrading Spring Squat Shearwall Spring Muscle Seatbelt Thermal Isotropic Thermal Orthotropic Thermal Isotropic (Temp Dependent) Thermal Orthotropic (Temp Dependent) Thermal Discrete Beam Thermal CWM (Welding) Thermal Orthotropic(Temp dep-load curve) Thermal Isotropic (Phase Change) Thermal Isotropic (Temp dep-load curve) Thermal User Defined Y Y Y Y Y Y Y Y Y Y Y Y Y Y Y Y Y Y Y Y Y Y Y Y Y Y FL FL FL FL CIV CIV BIO HT HT HT HT HT HT HT HT HT HT ALPHABETIZED MATERIALS LIST Alphabetized Materials List Material Keyword Number *EOS *EOS_GASKET *EOS_GRUNEISEN *EOS_IDEAL_GAS *EOS_IGNITION_AND_GROWTH_OF_REACTION_IN_HE *EOS_JWL *EOS_JWLB *EOS_LINEAR_POLYNOMIAL *EOS_LINEAR_POLYNOMIAL_WITH_ENERGY_LEAK *EOS_MIE_GRUNEISEN *EOS_PROPELLANT_DEFLAGRATION *EOS_RATIO_OF_POLYNOMIALS *EOS_SACK_TUESDAY *EOS_TABULATED *EOS_TABULATED_COMPACTION *EOS_TENSOR_PORE_COLLAPSE *EOS_USER_DEFINED *MAT_{OPTION}TROPIC_ELASTIC *MAT_1DOF_GENERALIZED_SPRING *MAT_3-PARAMETER_BARLAT *MAT_4A_MICROMEC *MAT_ACOUSTIC *MAT_ADD_AIRBAG_POROSITY_LEAKAGE *MAT_ADD_COHESIVE *MAT_ADD_EROSION *MAT_ADD_FATIGUE *MAT_ADD_GENERALIZED_DAMAGE *MAT_002 *MAT_146 *MAT_036 *MAT_215 *MAT_090 ALPHABETIZED MATERIALS LIST Material Keyword Number *MAT_ADD_PERMEABILITY *MAT_ADD_PORE_AIR *MAT_ADD_THERMAL_EXPANSION *MAT_ADHESIVE_CURING_VISCOELASTIC *MAT_ALE_GAS_MIXTURE *MAT_ALE_HERSCHEL *MAT_ALE_INCOMPRESSIBLE *MAT_ALE_MIXING_LENGTH *MAT_ALE_VACUUM *MAT_ALE_VISCOUS *MAT_AMORPHOUS_SOLIDS_FINITE_STRAIN *MAT_ANISOTROPIC_ELASTIC *MAT_ANISOTROPIC_ELASTIC_PLASTIC *MAT_ANISOTROPIC_PLASTIC *MAT_ANISOTROPIC_THERMOELASTIC *MAT_ANISOTROPIC_VISCOPLASTIC *MAT_ARRUDA_BOYCE_RUBBER *MAT_ARUP_ADHESIVE *MAT_BAMMAN *MAT_BAMMAN_DAMAGE *MAT_BARLAT_ANISOTROPIC_PLASTICITY *MAT_BARLAT_YLD2000 *MAT_BARLAT_YLD96 *MAT_BERGSTROM_BOYCE_RUBBER *MAT_BILKHU/DUBOIS_FOAM *MAT_BIOT_HYSTERETIC *MAT_BLATZ-KO_FOAM *MAT_BLATZ-KO_RUBBER *MAT_BOLT_BEAM *MAT_BRAIN_LINEAR_VISCOELASTIC *MAT_277 *MAT_ALE_02 *MAT_ALE_06 *MAT_160 *MAT_ALE_04 *MAT_ALE_01 *MAT_ALE_03 *MAT_256 *MAT_002_ANISO *MAT_157 *MAT_103_P *MAT_189 *MAT_103 *MAT_127 *MAT_169 *MAT_051 *MAT_052 *MAT_033 *MAT_133 *MAT_033_96 *MAT_269 *MAT_075 *MAT_232 *MAT_038 *MAT_007 *MAT_208 *MAT_164 ALPHABETIZED MATERIALS LIST Material Keyword Number *MAT_BRITTLE_DAMAGE *MAT_CABLE_DISCRETE_BEAM *MAT_CAZACU_BARLAT *MAT_CELLULAR_RUBBER *MAT_CF_MICROMECHANICS *MAT_CHRONOLOGICAL_VISCOELASTIC *MAT_CLOSED_CELL_FOAM *MAT_CODAM2 *MAT_COHESIVE_ELASTIC *MAT_COHESIVE_GENERAL *MAT_COHESIVE_MIXED_MODE *MAT_COHESIVE_MIXED_MODE_ELASTOPLASTIC_RATE *MAT_COHESIVE_PAPER *MAT_COHESIVE_TH *MAT_COMPOSITE_DAMAGE *MAT_COMPOSITE_DIRECT *MAT_COMPOSITE_DMG_MSC *MAT_COMPOSITE_FAILURE_{OPTION}_MODEL *MAT_COMPOSITE_LAYUP *MAT_COMPOSITE_MATRIX *MAT_COMPOSITE_MSC *MAT_COMPRF *MAT_CONCRETE_BEAM *MAT_CONCRETE_DAMAGE *MAT_CONCRETE_DAMAGE_PLASTIC_MODEL *MAT_CONCRETE_DAMAGE_REL3 *MAT_CONCRETE_EC2 *MAT_CORUS_VEGTER *MAT_CRUSHABLE_FOAM *MAT_CSCM_{OPTION} *MAT_096 *MAT_071 *MAT_233 *MAT_087 *MAT_278 *MAT_276 *MAT_053 *MAT_219 *MAT_184 *MAT_186 *MAT_138 *MAT_240 *MAT_279 *MAT_185 *MAT_022 *MAT_118 *MAT_162 *MAT_059 *MAT_116 *MAT_117 *MAT_161 *MAT_293 *MAT_195 *MAT_072 *MAT_273 *MAT_072R3 *MAT_172 *MAT_136 *MAT_063 *MAT_159 ALPHABETIZED MATERIALS LIST Material Keyword Number *MAT_CWM *MAT_DAMAGE_1 *MAT_DAMAGE_2 *MAT_DAMAGE_3 *MAT_DAMPER_NONLINEAR_VISCOUS *MAT_DAMPER_VISCOUS *MAT_DESHPANDE_FLECK_FOAM *MAT_DRUCKER_PRAGER *MAT_DRY_FABRIC *MAT_EIGHT_CHAIN_RUBBER *MAT_ELASTIC *MAT_ELASTIC_6DOF_SPRING_DISCRETE_BEAM *MAT_ELASTIC_FLUID *MAT_ELASTIC_PHASE_CHANGE *MAT_ELASTIC_PLASTIC_HYDRO_{OPTION} *MAT_ELASTIC_PLASTIC_THERMAL *MAT_ELASTIC_SPRING_DISCRETE_BEAM *MAT_ELASTIC_VISCOPLASTIC_THERMAL *MAT_ELASTIC_WITH_VISCOSITY *MAT_ELASTIC_WITH_VISCOSITY_CURVE *MAT_EMMI *MAT_ENHANCED_COMPOSITE_DAMAGE *MAT_EXTENDED_3-PARAMETER_BARLAT *MAT_FABRIC *MAT_FABRIC_MAP *MAT_FHWA_SOIL *MAT_FHWA_SOIL_NEBRASKA *MAT_FINITE_ELASTIC_STRAIN_PLASTICITY *MAT_FLD_3-PARAMETER_BARLAT *MAT_FLD_TRANSVERSELY_ANISOTROPIC *MAT_270 *MAT_104 *MAT_105 *MAT_153 *MAT_S05 *MAT_S02 *MAT_154 *MAT_193 *MAT_214 *MAT_267 *MAT_001 *MAT_093 *MAT_001_FLUID *MAT_216 *MAT_010 *MAT_004 *MAT_074 *MAT_106 *MAT_060 *MAT_060C *MAT_151 *MAT_054-055 *MAT_036E *MAT_034 *MAT_034M *MAT_147 *MAT_147_N *MAT_112 *MAT_190 *MAT_039 ALPHABETIZED MATERIALS LIST Material Keyword Number *MAT_FORCE_LIMITED *MAT_FRAZER_NASH_RUBBER_MODEL *MAT_FU_CHANG_FOAM *MAT_GAS_MIXTURE *MAT_GENERAL_JOINT_DISCRETE_BEAM *MAT_GENERAL_NONLINEAR_1DOF_DISCRETE_BEAM *MAT_GENERAL_NONLINEAR_6DOF_DISCRETE_BEAM *MAT_GENERAL_SPRING_DISCRETE_BEAM *MAT_GENERAL_VISCOELASTIC *MAT_GENERALIZED_PHASE_CHANGE *MAT_GEOLOGIC_CAP_MODEL *MAT_GEPLASTIC_SRATE_2000a *MAT_GLASS *MAT_GURSON *MAT_GURSON_JC *MAT_GURSON_RCDC *MAT_HEART_TISSUE *MAT_HIGH_EXPLOSIVE_BURN *MAT_HILL_3R *MAT_HILL_3R_3D *MAT_HILL_90 *MAT_HILL_FOAM *MAT_HONEYCOMB *MAT_HYDRAULIC_GAS_DAMPER_DISCRETE_BEAM *MAT_HYPERELASTIC_RUBBER *MAT_HYSTERETIC_REINFORCEMENT *MAT_HYSTERETIC_SOIL *MAT_INELASTC_6DOF_SPRING_DISCRETE_BEAM *MAT_INELASTIC_6DOF_SPRING_DISCRETE_BEAM *MAT_INELASTIC_SPRING_DISCRETE_BEAM *MAT_029 *MAT_031 *MAT_083 *MAT_148 *MAT_097 *MAT_121 *MAT_119 *MAT_196 *MAT_076 *MAT_254 *MAT_025 *MAT_101 *MAT_280 *MAT_120 *MAT_120_JC *MAT_120_RCDC *MAT_128 *MAT_008 *MAT_122 *MAT_122_3D *MAT_243 *MAT_177 *MAT_026 *MAT_070 *MAT_077_H *MAT_203 *MAT_079 *MAT_095 *MAT_095 *MAT_094 ALPHABETIZED MATERIALS LIST Material Keyword *MAT_INV_HYPERBOLIC_SIN(_THERMAL) *MAT_ISOTROPIC_ELASTIC_FAILURE *MAT_ISOTROPIC_ELASTIC_PLASTIC *MAT_ISOTROPIC_SMEARED_CRACK *MAT_JOHNSON_COOK *MAT_JOHNSON_HOLMQUIST_CERAMICS *MAT_JOHNSON_HOLMQUIST_CONCRETE *MAT_JOHNSON_HOLMQUIST_JH1 *MAT_JOINTED_ROCK *MAT_KELVIN-MAXWELL_VISCOELASTIC *MAT_KINEMATIC_HARDENING_BARLAT2000 *MAT_KINEMATIC_HARDENING_BARLAT89 Number *MAT_102(_T) *MAT_013 *MAT_012 *MAT_131 *MAT_015 *MAT_110 *MAT_111 *MAT_241 *MAT_198 *MAT_061 *MAT_242 *MAT_226 *MAT_KINEMATIC_HARDENING_TRANSVERSELY_ANISOTROPIC *MAT_125 *MAT_LAMINATED_COMPOSITE_FABRIC *MAT_LAMINATED_FRACTURE_DAIMLER_CAMANHO *MAT_LAMINATED_FRACTURE_DAIMLER_PINHO *MAT_LAMINATED_GLASS *MAT_LAYERED_LINEAR_PLASTICITY *MAT_LINEAR_ELASTIC_DISCRETE_BEAM *MAT_LOW_DENSITY_FOAM *MAT_LOW_DENSITY_SYNTHETIC_FOAM_{OPTION} *MAT_LOW_DENSITY_VISCOUS_FOAM *MAT_LUNG_TISSUE *MAT_MCCORMICK *MAT_MICROMECHANICS_DRY_FABRIC *MAT_MODIFIED_CRUSHABLE_FOAM *MAT_MODIFIED_FORCE_LIMITED *MAT_MODIFIED_HONEYCOMB *MAT_MODIFIED_JOHNSON_COOK *MAT_MODIFIED_PIECEWISE_LINEAR_PLASTICITY *MAT_058 *MAT_262 *MAT_261 *MAT_032 *MAT_114 *MAT_066 *MAT_057 *MAT_179 *MAT_073 *MAT_129 *MAT_167 *MAT_235 *MAT_163 *MAT_139 *MAT_126 *MAT_107 *MAT_123 ALPHABETIZED MATERIALS LIST Material Keyword *MAT_MODIFIED_ZERILLI_ARMSTRONG *MAT_MOHR_COULOMB *MAT_MOHR_NON_ASSOCIATED_FLOW *MAT_MOMENT_CURVATURE_BEAM *MAT_MOONEY-RIVLIN_RUBBER *MAT_MOONEY-RIVLIN_RUBBER_PHASE_CHANGE *MAT_MTS *MAT_MUSCLE *MAT_NONLINEAR_ELASTIC_DISCRETE_BEAM *MAT_NONLINEAR_ORTHOTROPIC *MAT_NONLINEAR_PLASTIC_DISCRETE_BEAM *MAT_NONLOCAL *MAT_NULL *MAT_OGDEN_RUBBER *MAT_OPTION_TROPIC_ELASTIC *MAT_OPTION_TROPIC_ELASTIC_PHASE_CHANGE *MAT_ORIENTED_CRACK *MAT_ORTHO_ELASTIC_PLASTIC *MAT_ORTHOTROPIC_SIMPLIFIED_DAMAGE *MAT_ORTHOTROPIC_SMEARED_CRACK *MAT_ORTHOTROPIC_THERMAL *MAT_ORTHOTROPIC_VISCOELASTIC *MAT_PAPER *MAT_PERT_PIECEWISE_LINEAR_PLASTICITY *MAT_PHS_BMW *MAT_PIECEWISE_LINEAR_PLASTIC_THERMAL *MAT_PIECEWISE_LINEAR_PLASTICITY *MAT_PITZER_CRUSHABLE_FOAM *MAT_PLASTIC_GREEN-NAGHDI_RATE *MAT_PLASTIC_KINEMATIC Number *MAT_065 *MAT_173 *MAT_260B *MAT_166 *MAT_027 *MAT_218 *MAT_088 *MAT_156 *MAT_067 *MAT_040 *MAT_068 *MAT_009 *MAT_077_O *MAT_002 *MAT_217 *MAT_017 *MAT_108 *MAT_221 *MAT_132 *MAT_021 *MAT_086 *MAT_274 *MAT_238 *MAT_248 *MAT_255 *MAT_024 *MAT_144 *MAT_035 *MAT_003 ALPHABETIZED MATERIALS LIST Material Keyword Number *MAT_PLASTIC_NONLINEAR_KINEMATIC *MAT_PLASTIC_NONLINEAR_KINEMATIC_B *MAT_PLASTICITY_COMPRESSION_TENSION *MAT_PLASTICITY_COMPRESSION_TENSION_EOS *MAT_PLASTICITY_POLYMER *MAT_PLASTICITY_WITH_DAMAGE *MAT_165 *MAT_165B *MAT_124 *MAT_155 *MAT_089 *MAT_081 *MAT_PLASTICITY_WITH_DAMAGE_ORTHO(_RCDC) *MAT_082(_RCDC) *MAT_PML_{OPTION}TROPIC_ELASTIC *MAT_PML_ACOUSTIC *MAT_PML_ELASTIC *MAT_PML_ELASTIC_FLUID *MAT_PML_HYSTERETIC *MAT_PML_NULL *MAT_POLYMER *MAT_POWDER *MAT_POWER_LAW_PLASTICITY *MAT_PSEUDO_TENSOR *MAT_QUASILINEAR_VISCOELASTIC *MAT_RAMBERG-OSGOOD *MAT_RATE_SENSITIVE_COMPOSITE_FABRIC *MAT_RATE_SENSITIVE_POLYMER *MAT_RATE_SENSITIVE_POWERLAW_PLASTICITY *MAT_RC_BEAM *MAT_RC_SHEAR_WALL *MAT_REINFORCED_THERMOPLASTIC *MAT_REINFORCED_THERMOPLASTIC_UDFIBER *MAT_RESULTANT_ANISOTROPIC *MAT_RESULTANT_PLASTICITY *MAT_RHT LS-DYNA R10.0 *MAT_245 *MAT_231 *MAT_230 *MAT_230 *MAT_237 *MAT_246 *MAT_168 *MAT_271 *MAT_018 *MAT_016 *MAT_176 *MAT_080 *MAT_158 *MAT_141 *MAT_064 *MAT_174 *MAT_194 *MAT_249 *MAT_249_ UDFIBER *MAT_170 *MAT_028 ALPHABETIZED MATERIALS LIST Material Keyword Number *MAT_RIGID *MAT_RIGID_DISCRETE *MAT_SAMP-1 *MAT_SCC_ON_RCC *MAT_SCHWER_MURRAY_CAP_MODEL *MAT_SEATBELT *MAT_SEISMIC_BEAM *MAT_SEISMIC_ISOLATOR *MAT_SHAPE_MEMORY *MAT_SID_DAMPER_DISCRETE_BEAM *MAT_SIMPLIFIED_JOHNSON_COOK *MAT_020 *MAT_220 *MAT_187 *MAT_236 *MAT_145 *MAT_B01 *MAT_191 *MAT_197 *MAT_030 *MAT_069 *MAT_098 *MAT_SIMPLIFIED_JOHNSON_COOK_ORTHOTROPIC_DAMAGE *MAT_099 *MAT_SIMPLIFIED_RUBBER/FOAM_{OPTION} *MAT_SIMPLIFIED_RUBBER_WITH_DAMAGE *MAT_SMOOTH_VISCOELASTIC_VISCOPLASTIC *MAT_SOFT_TISSUE *MAT_SOFT_TISSUE_VISCO *MAT_SOIL_AND_FOAM *MAT_SOIL_AND_FOAM_FAILURE *MAT_SOIL_BRICK *MAT_SOIL_CONCRETE *MAT_SPECIAL_ORTHOTROPIC *MAT_SPH_VISCOUS *MAT_SPOTWELD_{OPTION} *MAT_SPOTWELD_DAIMLERCHRYSLER *MAT_SPR_JLR *MAT_SPRING_ELASTIC *MAT_SPRING_ELASTOPLASTIC *MAT_SPRING_GENERAL_NONLINEAR *MAT_SPRING_INELASTIC *MAT_181 *MAT_183 *MAT_275 *MAT_091 *MAT_092 *MAT_005 *MAT_014 *MAT_192 *MAT_078 *MAT_130 *MAT_SPH_01 *MAT_100 *MAT_100_DA *MAT_211 *MAT_S01 *MAT_S03 *MAT_S06 *MAT_S08 ALPHABETIZED MATERIALS LIST Material Keyword Number *MAT_SPRING_MAXWELL *MAT_SPRING_MUSCLE *MAT_SPRING_NONLINEAR_ELASTIC *MAT_SPRING_SQUAT_SHEARWALL *MAT_SPRING_TRILINEAR_DEGRADING *MAT_STEEL_CONCENTRIC_BRACE *MAT_STEEL_EC3 *MAT_STEINBERG *MAT_STEINBERG_LUND *MAT_STOUGHTON_NON_ASSOCIATED_FLOW *MAT_STRAIN_RATE_DEPENDENT_PLASTICITY *MAT_TABULATED_JOHNSON_COOK *MAT_S07 *MAT_S15 *MAT_S04 *MAT_S14 *MAT_S13 *MAT_171 *MAT_202 *MAT_011 *MAT_011_LUND *MAT_260A *MAT_019 *MAT_224 *MAT_TABULATED_JOHNSON_COOK_GYS *MAT_224_GYS *MAT_TABULATED_JOHNSON_COOK_ORTHO_PLASTICITY *MAT_264 *MAT_TAILORED_PROPERTIES *MAT_TEMPERATURE_DEPENDENT_ORTHOTROPIC *MAT_THERMAL_CHEMICAL_REACTION *MAT_THERMAL_CWM *MAT_THERMAL_DISCRETE_BEAM *MAT_THERMAL_ISOTROPIC *MAT_THERMAL_ISOTROPIC_PHASE_CHANGE *MAT_THERMAL_ISOTROPIC_TD *MAT_THERMAL_ISOTROPIC_TD_LC *MAT_THERMAL_OPTION *MAT_THERMAL_ORTHOTROPIC *MAT_THERMAL_ORTHOTROPIC_TD *MAT_THERMAL_ORTHOTROPIC_TD_LC *MAT_THERMAL_USER_DEFINED *MAT_THERMO_ELASTO_VISCOPLASTIC_CREEP *MAT_TISSUE_DISPERSED LS-DYNA R10.0 *MAT_251 *MAT_023 *MAT_T06 *MAT_T07 *MAT_T05 *MAT_TO1 *MAT_T09 *MAT_T03 *MAT_T10 *MAT_T00 *MAT_T02 *MAT_T04 *MAT_T08 *MAT_T11 *MAT_188 ALPHABETIZED MATERIALS LIST Material Keyword *MAT_TOUGHENED_ADHESIVE_POLYMER Number *MAT_252 *MAT_TRANSVERSELY_ANISOTROPIC_ELASTIC_PLASTIC *MAT_037 *MAT_TRANSVERSELY_ISOTROPIC_CRUSHABLE_FOAM *MAT_TRIP *MAT_UHS_STEEL *MAT_UNIFIED_CREEP *MAT_UNIFIED_CREEP_ORTHO *MAT_USER_DEFINED_MATERIAL_MODELS *MAT_VACUUM *MAT_VISCOELASTIC *MAT_VISCOELASTIC_FABRIC *MAT_VISCOELASTIC_HILL_FOAM *MAT_VISCOELASTIC_LOOSE_FABRIC *MAT_VISCOELASTIC_THERMAL *MAT_VISCOPLASTIC_MIXED_HARDENING *MAT_VISCOUS_FOAM *MAT_142 *MAT_113 *MAT_244 *MAT_115 *MAT_115_O *MAT_041-050 *MAT_140 *MAT_006 *MAT_134 *MAT_178 *MAT_234 *MAT_175 *MAT_225 *MAT_062 *MAT_WINFRITH_CONCRETE_REINFORCEMENT *MAT_084_REINF *MAT_WINFRITH_CONCRETE *MAT_WOOD_{OPTION} *MAT_WTM_STM *MAT_WTM_STM_PLC *MAT_084 *MAT_143 *MAT_135 *MAT_135_PLC *MAT_ADD_AIRBAG_POROSITY_LEAKAGE This command allows users to model porosity leakage through non-fabric material when such material is used as part of control volume, airbag. It applies to both *AIRBAG_HYBRID and *AIRBAG_WANG_NEFSKE. Card 1 1 2 3 4 5 Variable MID FLC/X2 FAC/X3 ELA FVOPT Type I F F F F 8 6 X0 F 7 X1 F Default none none 1.0 none none none none VARIABLE DESCRIPTION MID Material ID for which the porosity leakage property applies FLC/X2 If X0≠0 and X0≠1 X2 is one of the coefficients of the porosity in the equation of Anagonye and Wang [1999]. (Defined below in description for X0/X1) If X0=0 GE.0.0: X2, in this context named FLC, is an optional fabric porous leakage flow coefficient. LT.0.0: |FLC| is the load curve ID of the curve defining FLC versus time. If X0=1 GE.0.0: See X0=0 above. LT.0.0: |FLC| is the load curve ID defining FLC versus the stretching ratio defined as 𝑟𝑠 = 𝐴/𝐴0. See notes below. FAC/X3 If X0 ≠ 0 and X0 ≠ 1 X3 is one of the coefficients of the porosity in the equation of Anagonye and Wang [1999]. (Defined below in description for X0/X1) If X0 = 0 and FVOPT < 7 GE.0.0: X3, in this context named FAC, is an optional fabric characteristic parameter. LT.0.0: |FAC| is the load curve ID of the curve defining FAC versus absolute pressure. If X0 = 1 and FVOPT < 7 GE.0.0: See X0 = 0 and FVOPT < 7 above. LT.0.0: |FAC| is the load curve ID defining FAC versus the pressure ratio defined as 𝑟𝑝 = 𝑃air/𝑃bag. See remark 3 of *MAT_FABRIC. If (X0 = 0 or X0 = 1) and (FVOPT = 7 or FVOPT = 8) GE.0.0: See X0 = 0 and FVOPT < 7 above. LT.0.0: FAC defines leakage volume flux rate versus absolute pressure. The volume flux (per area) rate (per time) has the unit of velocity and it is equivalent to relative porous gas speed. [ 𝑑(Volflux) 𝑑𝑡 ] = [volume] [area] [time] = [length] [time] = [velocity], ELA Effective leakage area for blocked fabric, ELA. LT.0.0: |ELA| is the load curve ID of the curve defining ELA versus time. The default value of zero assumes that no leakage occurs. A value of .10 would assume that 10% of the blocked fabric is leaking gas. FVOPT Fabric venting option. EQ.1: Wang-Nefske formulas for venting through an orifice are used. Blockage is not considered. EQ.2: Wang-Nefske formulas for venting through an orifice are used. Blockage of venting area due to contact is consid- ered. EQ.3: Leakage formulas of Graefe, Krummheuer, and Siejak [1990] are used. Blockage is not considered. EQ.4: Leakage formulas of Graefe, Krummheuer, and Siejak [1990] are used. Blockage of venting area due to contact is considered. EQ.5: Leakage formulas based on flow through a porous media are used. Blockage is not considered. EQ.6: Leakage formulas based on flow through a porous media are used. Blockage of venting area due to contact is con- sidered. EQ.7: Leakage is based on gas volume outflow versus pressure load curve [Lian, 2000]. Blockage is not considered. Absolute pressure is used in the porous-velocity-versus- pressure load curve, given as FAC. EQ.8: Leakage is based on gas volume outflow versus pressure load curve [Lian 2000]. Blockage of venting or porous area due to contact is considered. Absolute pressure is used in the porous-velocity-versus-pressure load curve, given as FAC. X0, X1 Coefficients of Anagonye and Wang [1999] porosity equation for the leakage area: 𝐴leak = 𝐴0(𝑋0 + 𝑋1𝑟𝑠 + 𝑋2𝑟𝑝 + 𝑋3𝑟𝑠𝑟𝑝) *MAT_ADD_COHESIVE The ADD_COHESIVE option offers the possibility to use a selection of 3-dimensional material models in LS-DYNA in conjunction with cohesive elements. Usually the cohesive elements (ELFORM = 19 and 20 of *SECTION_SOLID) can only be used with a small subset of materials (41-50, 138, 184, 185, 186, 240). But with this additional keyword, a bigger amount of standard 3-d material models can be used, that would only be available for solid elements in general. Currently the following material models are supported: 1, 3, 4, 6, 15, 24, 41-50, 81, 82, 89, 96, 98, 103, 104, 105, 106, 107, 115, 120, 123, 124, 141, 168, 173, 187, 188, 193, 224, 225, 252, and 255. Card 1 1 2 3 4 5 6 7 8 Variable PID ROFLG INTFAIL THICK Type I F F F Default none 0.0 0.0 0.0 VARIABLE DESCRIPTION PID Part ID for which the cohesive property applies. ROFLG Flag for whether density is specified per unit area or volume. EQ.0.0: Density specified per unit volume (default). EQ.1.0: Density specified per unit area for controlling the mass of cohesive elements with an initial volume of zero. INTFAIL The number of integration points required for the cohesive element to be deleted. If it is zero, the element won’t be deleted even if it satisfies the failure criterion. The value of INTFAIL may range from 1 to 4, with 1 the recommended value. THICK Thickness of the adhesive layer. EQ.0.0: The actual thickness of the cohesive element is used. GT.0.0: User specified thickness. *MAT Cohesive elements possess 3 kinematic variables, namely two relative displacements 𝛿1, 𝛿2 in tangential directions and one relative displacement 𝛿3 in normal direction. In a corresponding constitutive model, they are used to compute 3 associated traction stresses 𝑡1, 𝑡2, and 𝑡3, e.g. in the elastic case (*MAT_COHESIVE_ELASTIC): 𝑡1 ⎤ = ⎡ 𝑡2 ⎥ ⎢ 𝑡3⎦ ⎣ 𝐸𝑇 ⎡ ⎢ ⎣ 𝐸𝑇 ⎤ ⎥ 𝐸𝑁⎦ 𝛿1 ⎤ ⎡ 𝛿2 ⎥ ⎢ 𝛿3⎦ ⎣ On the other hand, hypoelastic 3-d material models for standard solid elements are formulated with respect to 6 independent strain rates and 6 associated stress rates, e.g. for isotropic elasticity (*MAT_ELASTIC): 𝜎̇𝑥𝑥 ⎤ ⎡ 𝜎̇𝑦𝑦 ⎥ ⎢ ⎥ ⎢ 𝜎̇𝑧𝑧 ⎥ ⎢ 𝜎̇𝑥𝑦 ⎥ ⎢ ⎥ ⎢ 𝜎̇𝑦𝑧 ⎥ ⎢ 𝜎̇𝑧𝑥⎦ ⎣ = (1 + 𝜈)(1 − 2𝜈) 1 − 𝜈 ⎡ ⎢ ⎢ ⎢ ⎢ ⎢ ⎣ 1 − 𝜈 1 − 𝜈 1 − 2𝜈 1 − 2𝜈 ⎤ ⎥ ⎥ ⎥ ⎥ ⎥ 1 − 2𝜈⎦ 𝜀̇𝑥𝑥 ⎤ ⎡ 𝜀̇𝑦𝑦 ⎥ ⎢ ⎥ ⎢ 𝜀̇𝑧𝑧 ⎥ ⎢ 𝜀̇𝑥𝑦 ⎥ ⎢ ⎥ ⎢ 𝜀̇𝑦𝑧 ⎥ ⎢ 𝜀̇𝑧𝑥⎦ ⎣ To be able to use such 3-dimensional material models in a cohesive element environment, an assumption is necessary to transform 3 relative displacements to 6 strain rates. Therefore it is assumed that no lateral expansion and no in-plane shearing is possible for the cohesive element: 𝛿1 ⎤ ⎡ 𝛿2 ⎥ ⎢ 𝛿3⎦ ⎣ → 𝜀̇𝑥𝑥 ⎤ ⎡ 𝜀̇𝑦𝑦 ⎥ ⎢ ⎥ ⎢ 𝜀̇𝑧𝑧 ⎥ ⎢ 𝜀̇𝑥𝑦 ⎥ ⎢ ⎥ ⎢ 𝜀̇𝑦𝑧 ⎥ ⎢ 𝜀̇𝑧𝑥⎦ ⎣ = ⎤ ⎡ ⎥ ⎢ 𝛿 ̇ ⎥ ⎢ 3/(𝑡 + 𝛿3) ⎥ ⎢ ⎥ ⎢ ⎥ ⎢ 𝛿 ̇ 2/(𝑡 + 𝛿3) ⎥ ⎢ 𝛿 ̇ 1/(𝑡 + 𝛿3)⎦ ⎣ where 𝑡 is the initial thickness of the adhesive layer, see parameter THICK. These strain rates are then used in a 3-d constitutive model to obtain new Cauchy stresses, where 3 components can finally be used for the cohesive element: 𝜎𝑥𝑥 ⎤ ⎡ 𝜎𝑦𝑦 ⎥ ⎢ 𝜎𝑧𝑧 ⎥ ⎢ ⎥ ⎢ 𝜎𝑥𝑦 ⎥ ⎢ 𝜎𝑦𝑧 ⎥ ⎢ 𝜎𝑧𝑥⎦ ⎣ → 𝑡1 ⎤ = ⎡ 𝑡2 ⎥ ⎢ 𝑡3⎦ ⎣ 𝜎𝑧𝑥 ⎥⎤ ⎢⎡ 𝜎𝑦𝑧 𝜎𝑧𝑧⎦ ⎣ If this keyword is used in combination with a 3-dimensional material model, the output to D3PLOT or ELOUT is organized as in other material models for cohesive elements, see e.g. *MAT_184. Instead of the usual six stress components, three traction stresses are written into those databases. The in-plane shear traction along the 1-2 edge replaces the x-stress, the orthogonal in-plane shear traction replaces the y-stress, and the traction in the normal direction replaces the z-stress. *MAT Many of the constitutive models in LS-DYNA do not allow failure and erosion. The ADD_EROSION option provides a way of including failure in these models. This option can also be applied to constitutive models that already include other failure/erosion criterion. For the non-damage options, each of the failure criteria defined here are applied independently, and once a sufficient number of those criteria are satisfied according to NCS, the element is deleted from the calculation. In addition to erosion, the “generalized incremental stress-state dependent damage model” (GISSMO) or alternative “damage initiation and evolution models” (DIEM) are available as described in the remarks. See variable IDAM. For DIEM, NCS has a special meaning, see description below for details. This option applies to nonlinear element formulations including the 2D continuum elements, 3D solid elements, 2D and 3D SPH particles, 3D shell elements, and thick shell elements. Beam formulations 1 and 11 currently support the erosion but not the damage and evolution models. NOTE: that all *MAT_ADD_EROSION commands in a model can be disabled by using *CONTROL_MAT. Card 1 1 2 3 4 5 6 7 8 Variable MID EXCL MXPRES MNEPS EFFEPS VOLEPS NUMFIP NCS Type A8 F F F F F F F Default none none 0.0 0.0 0.0 0.0 1.0 1.0/0.0 Card 2 1 2 3 4 5 6 7 8 Variable MNPRES SIGP1 SIGVM MXEPS EPSSH SIGTH IMPULSE FAILTM Type F F F F F F F F Default none none none none none none none none *MAT_ADD_EROSION Card 3 1 2 3 4 5 6 7 8 Variable IDAM DMGTYP LCSDG ECRIT DMGEXP DCRIT FADEXP LCREGD Type A8 F F F F F F F Default 0.0 0.0 0.0 0.0 1.0 0.0 1.0 0.0 Additional card for IDAM > 0. Card 4 1 2 3 4 5 6 7 8 Variable SIZFLG REFSZ NAHSV LCSRS SHRF BIAXF Type F F F F F F Default 0.0 0.0 0.0 0.0 0.0 0.0 Damage Initiation and Evolution Card Pairs. For IDAM < 0 include | IDAM | pairs of Cards 5 and 6. 5 6 7 8 Card 5 1 Variable DITYP Type F 2 P1 F 3 P2 F 4 P3 F Default 0.0 0.0 0.0 0.0 6 7 8 *MAT_ADD_EROSION Card 6 1 2 Variable DETYP DCTYP Type F F 3 Q1 F 4 Q2 F Default 0.0 0.0 0.0 0.0 Optional Card with additional failure criteria. Card 7 1 2 3 4 5 6 7 8 Variable LCFLD EPSTHIN ENGCRT RADCRT Type F F F F Default 0.0 0.0 0.0 0.0 VARIABLE MID EXCL DESCRIPTION Material identification for which this erosion definition applies. A unique number or label not exceeding 8 characters must be specified. The exclusion number, which applies to the failure values defined on Cards 1, 2, and 7. When any of the failure values on these cards are set to the exclusion number, the associated failure criterion is not invoked. Or in other words, only the failure values not set to the exclusion number are invoked. The default value of EXCL is 0.0, which eliminates all failure criteria from consideration that have their constants left blank or set to 0.0. As an example, to prevent a material from developing tensile pressure, the user could specify an unusual value for the exclusion number, e.g., 1234, set MNPRES to 0.0, and set all the remaining failure values to 1234. However, use of an exclusion number may be considered nonessential since the same effect could be achieved without use of the exclusion number by setting MNPRES to a very small negative value. MXPRES *MAT_ADD_EROSION DESCRIPTION Maximum pressure at failure, 𝑃max. If the value is exactly zero, it is automatically excluded to maintain compatibility with old input files. MNEPS Minimum principal strain at failure, 𝜀min. If the value is exactly zero, it is automatically excluded to maintain compatibility with old input files. EFFEPS Maximum effective strain at failure: 𝜀eff = ∑ √ 𝑖𝑗 dev𝜀𝑖𝑗 𝜀𝑖𝑗 dev . If the value is exactly zero, it is automatically excluded to maintain compatibility with old input files. If the value is negative, then |EFFEPS| is the effective plastic strain to failure. In combination with cohesive elements, EFFEPS is the maximum effective in-plane strain. VOLEPS Volumetric strain at failure, or 𝜀vol = 𝜀11 + 𝜀22 + 𝜀33, ln(relative volume). VOLEPS can be a positive or negative number depending on whether the failure is in tension or compression, respectively. If the value is exactly zero, it is automatically excluded to maintain compatibility with old input files. VARIABLE NUMFIP DESCRIPTION Number of failed integration points prior to element deletion. The default is unity. See Remark 10. LT.0.0 (IDAM = 0): Only is for shells. |NUMFIP| the percentage of integration points which must exceed the failure criterion before element fails. If NUMFIP < -100, then |NUMFIP|- 100 is the number of failed integration points prior to element deletion. LT.0.0 (IDAM≠ 0): Only is for shells. |NUMFIP| the percentage of layers which must fail before element fails. For shell formulations with 4 integration points per layer, the layer is con- sidered failed if any of the integration points in the layer fails. NCS This meaning of this input depends on whether the damage option DIEM is used or not. IDAM.GE.0: Number of failure conditions to satisfy before failure occurs. For example, if SIGP1 and SIGVM are defined and if NCS = 2, both failure criteria must be met before element deletion can occur. The default is set to unity. IDAM.LT.0: Plastic strain increment between evaluation of damage instability and evolution criteria. See DI- EM description, the default is zero. MNPRES Minimum pressure at failure, 𝑃min. SIGP1 SIGVM MXEPS EPSSH SIGTH Principal stress at failure, 𝜎max. Equivalent stress at failure, 𝜎̅̅̅̅̅max. The equivalent stress at failure is made a function of the effective strain rate by setting SIGVM to the negative of the appropriate load curve ID. Maximum principal strain at failure, 𝜀max. The maximum principal strain at failure is made a function of the effective strain rate by setting MXEPS to the negative of the appropriate load curve ID. Tensorial shear strain at failure, 𝛾max/2. Threshold stress, 𝜎0. *MAT_ADD_EROSION DESCRIPTION IMPULSE Stress impulse for failure, 𝐾f. FAILTM Failure time. When the problem time exceeds the failure time, the material is removed. IDAM Flag for damage model. EQ.0: no damage model is used. EQ.1: GISSMO damage model. LT.0: -IDAM represents the number of damage initiation and evolution model (DIEM) criteria to be applied DMGTYP For GISSMO damage type the following applies. DMGTYP is interpreted digit-wise as follows: DMGTYP = [𝑁𝑀] = 𝑀 + 10 × 𝑁 M.EQ.0: Damage is accumulated, no coupling to flow stress, no failure. M.EQ.1: Damage is accumulated, element failure occurs for 𝐷 = 1. Coupling of damage to flow stress depending on parameters, see remarks below. N.EQ.0: Equivalent plastic strain is the driving quantity for the damage. (To be more precise, it’s the history variable that LS-PrePost blindly labels as “plastic strain”. What this history variable actually represents depends on the material model.) N.GT.0: The Nth additional history variable is the driving quantity for damage. These additional history varri- ables are the same ones flagged by the *DATABASE_- EXTENT_BINARY keyword’s NEIPS and NEIPH fields. For example, for solid elements with *MAT_- 187 setting 𝑁 = 6 chooses volumetric plastic strain as the driving quantity for the GISSMO damage. For IDAM.LT.0 the following applies. EQ.0: No action is taken EQ.1: Damage history is initiated based on values of initial plastic strains and initial strain tensor, this is to be used in multistage analyses VARIABLE LCSDG DESCRIPTION Load curve ID or Table ID. Load curve defines equivalent plastic strain to failure vs. triaxiality. Table defines for each Lode parameter value (between -1 and 1) a load curve ID giving the equivalent plastic strain to failure vs. triaxiality for that Lode parameter value. ECRIT Critical plastic strain (material instability), see below. LT.0.0: |ECRIT| is either a load curve ID defining critical equivalent plastic strain versus triaxiality or a table ID defining critical equivalent plastic strain as a function of triaxiality and Lode parameter (as in LCSDG). EQ.0.0: Fixed value DCRIT defining critical damage is read GT.0.0: Fixed value for stress-state independent critical equivalent plastic strain. DMGEXP Exponent for nonlinear damage accumulation, see remarks. DCRIT Damage threshold value (critical damage). If a Load curve of critical plastic strain or fixed value is given by ECRIT, input is ignored. FADEXP Exponent for damage-related stress fadeout. LCREGD LT.0.0: |FADEXP| is load curve ID defining element-size dependent fading exponent. GT.0.0: Constant fading exponent. Load curve ID defining element size dependent regularization factors for equivalent plastic strain to failure in the GISSMO damage model. This feature can also be used with the standard (non-GISSMO) failure criteria of Cards 1 (MXPRES, MNEPS, EFFEPS, VOLEPS), 2 (MNPRES, SIGP1, SIGVM, MXEPS, EPSSH, IMPULSE) and 4 (LCFLD, EPSTHIN), i.e. when IDAM = 0. *MAT_ADD_EROSION DESCRIPTION SIZFLG Flag for method of element size determination. EQ.0: (default) Element size is determined in undeformed configuration as square root of element area (shells), or cubic root of element volume (solids), respectively. EQ.1: Element size is updated every time step, and determined as mean edge length (this option was added to ensure comparability with *MAT_120, and is not recommended for general purpose). Reference element size, for which an additional output of damage will be generated. This is necessary to ensure the applicability of resulting damage quantities when transferred to different mesh sizes. Number of history variables from damage model which should be stored in standard material history array for Postprocessing. See remarks. Load curve ID defining failure strain scaling factor for LCSDG vs. strain rate. If the first strain rate value in the curve is negative, it is assumed that all strain rate values are given as natural logarithm of the strain rate. The curve should not extrapolate to zero or failure may occur at low strain. GT.0: scale ECRIT, too LT.0: do not scale ECRIT. Reduction factor for regularization at triaxiality = 0 (shear) Reduction factor for regularization at triaxiality = 2/3 (biaxial) Damage initiation type EQ.0.0: Ductile based on stress triaxiality EQ.1.0: Shear EQ.2.0: MSFLD EQ.3.0: FLD REFSZ NAHSV LCSRS SHRF BIAXF DITYP EQ.4.0: Ductile based on normalized principal stress P1 Damage initiation parameter DITYP.EQ.0.0: Load curve/table ID representing plastic strain VARIABLE DESCRIPTION at onset of damage as function of stress triaxiali- ty 𝜂 and optionally plastic strain rate. DITYP.EQ.1.0: Load curve/table ID representing plastic strain at onset of damage as function of shear influ- ence 𝜃 and optionally plastic strain rate. DITYP.EQ.2.0: Load curve/table ID representing plastic strain at onset of damage as function of ratio of prin- cipal plastic strain rates 𝛼 and optionally plastic strain rate. DITYP.EQ.3.0: Load curve/table ID representing plastic strain at onset of damage as function of ratio of prin- cipal plastic strain rates 𝛼 and optionally plastic strain rate. DITYP.EQ.4.0: Load curve/table ID representing plastic strain at onset of damage as function of stress state pa- rameter 𝛽 and optionally plastic strain rate. P2 Damage initiation parameter DITYP.EQ.0.0: Not used DITYP.EQ.1.0: Pressure influence parameter 𝑘𝑠 DITYP.EQ.2.0: Layer specification EQ.0: Mid layer EQ.1: Outer layer DITYP.EQ.3.0: Layer specification EQ.0: Mid layer EQ.1: Outer layer DITYP.EQ.4.0: Triaxiality influence parameter 𝑘𝑑 P3 Damage initiation parameter DITYP.EQ.0.0: Not used DITYP.EQ.1.0: Not used DITYP.EQ.2.0: Initiation formulation EQ.0: Direct EQ.1: Incremental DITYP.EQ.3.0: Initiation formulation EQ.0: Direct DESCRIPTION EQ.1: Incremental DITYP.EQ.4.0: Not used *MAT_ADD_EROSION DETYP Damage evolution type EQ.0.0: Linear softening, evolution of damage is a function of the plastic displacement after the initiation of damage. EQ.1.0: Linear softening, evolution of damage is a function of the fracture energy after the initiation of damage. DCTYP Damage composition option for multiple criteria EQ.-1.0: Damage not coupled to stress EQ.0.0: Maximum EQ.1.0: Multiplicative Q1 Damage evolution parameter DETYP.EQ.0.0: Plastic displacement at failure, 𝑢𝑓 value corresponds to a table ID for 𝑢𝑓 tion of triaxiality and damage. 𝑝, a negative 𝑝 as a func- Q2 LCFLD DETYP.EQ.1.0: Fracture energy at failure, 𝐺𝑓 . Set to 1.0 to output information to log files (messag and d3hsp) when an integration point fails. Load curve ID or Table ID. Load curve defines the Forming Limit Diagram, where minor engineering strains in percent are defined as abscissa values and major engineering strains in percent are defined as ordinate values. Table defines for each strain rate an associated FLD curve. The forming limit diagram is shown in Figure M39-1. In defining the curve, list pairs of minor and major strains starting with the left most point and ending with the right most point. This criterion is only available for shell elements. EPSTHIN Thinning strain at failure for thin and thick shells. GT.0.0: individual thinning for each integration point from 𝑧- strain LT.0.0: averaged thinning strain from element thickness change VARIABLE DESCRIPTION ENGCRT Critical energy for nonlocal failure criterion, see Item 9 below. RADCRT Critical radius for nonlocal failure criterion, see Item 9 below. In addition to failure time, supported criteria for failure are: 1. 𝑃 ≥ 𝑃max, where P is the pressure (positive in compression), and 𝑃max is the maximum pressure at failure. 2. 𝜀3 ≤ 𝜀min, where 𝜀3 is the minimum principal strain, and 𝜀min is the minimum principal strain at failure. 3. 𝑃 ≤ 𝑃min, where P is the pressure (positive in compression), and 𝑃min is the minimum pressure at failure. 4. 𝜎1 ≥ 𝜎max, where 𝜎1 is the maximum principal stress, and 𝜎maxis the maximum principal stress at failure. 5. √3 ′ 𝜎𝑖𝑗 2 𝜎𝑖𝑗 ′ ≥ 𝜎̅̅̅̅̅max, where 𝜎𝑖𝑗 equivalent stress at failure. ′ are the deviatoric stress components, and 𝜎̅̅̅̅̅max is the 6. 𝜀1 ≥ 𝜀max, where 𝜀1 is the maximum principal strain, and 𝜀max is the maximum principal strain at failure. 7. 𝛾1 ≥ 𝛾max/2, where 𝛾1 is the maximum tensorial shear strain = (𝜀1 − 𝜀3)/2, and 𝛾max is the engineering shear strain at failure. 8. The Tuler-Butcher criterion, ∫ [max(0, 𝜎1 − 𝜎0)]2dt ≥ Kf, where 𝜎1 is the maximum principal stress, 𝜎0 is a specified threshold stress, 𝜎1 ≥ 𝜎0 ≥ 0, and Kf is the stress impulse for failure. Stress values below the threshold value are too low to cause fracture even for very long duration load- ings. 9. A nonlocal failure criterion which is mainly intended for windshield impact can be defined via ENGCRT, RADCRT, and one additional “main” failure criterion (only SIGP1 is available at the moment). All three parameters should be de- fined for one part, namely the windshield glass and the glass should be discre- tized with shell elements. The course of events of this nonlocal failure model is as follows: If the main failure criterion SIGP1 is fulfilled, the corresponding element is flagged as center of impact, but no element erosion takes place yet. Then, the internal energy of shells inside a circle, defined by RADCRT, around the center of impact is tested against the product of the given critical energy ENGCRT and the “area factor”. The area factor is defined as, Area Factor = total area of shell elements found inside the circle 2𝜋 × RADCRT2 The reason for having two times the circle area in the denominator is that we expect two layers of shell elements, as would typically be the case for laminated windshield glass.. If this energy criterion is exceeded, all elements of the part are now allowed to be eroded by the main failure criterion. 10. When IDAM = 0, there are 3 ways to specify how shell elements are eroded and removed from the calculation. a) When NUMFIP > 0, elements erode when NUMFIP points fail. b) When -100 ≤ NUMFIP < 0, elements erode when |NUMFIP| percent of the integration points fail. c) When NUMFIP < -100, elements erode when |NUMFIP|-100 integration points fail. For NUMFIP > 0 and -100 ≤ NUMFIP < 0, layers retain full strength until the element is eroded. For NUMFIP < -100, the stress at an integration point im- mediately drops to zero when failure is detected at that integration point. When IDAM ≠ 0, there are 2 ways to specify how shell elements are eroded and removed from the calculation. a) When NUMFIP > 0, elements erode when NUMFIP points fail. b) When NUMFIP < 0, elements erode when |NUMFIP| percent of the lay- ers fail. A layer fails if any integration point within that layer fails. When IDAM = 0, erosion is in terms of failed points, not layers. plastic failure strain compression -2/3 -1/3 tension 1/3 2/3 triaxiality h/σ vm Figure 2-1. Typical failure curve for metal sheet, modeled with shell elements. DAMAGE MODELS GISSMO: The GISSMO damage model is a phenomenological formulation that allows for an incremental description of damage accumulation, including softening and failure. It is intended to provide a maximum in variability for the description of damage for a variety of metallic materials (e.g. *MAT_024, *MAT_036, *MAT_103, …). The input of parameters is based on tabulated data, allowing the user to directly convert test data to numerical input. The model is based on an incremental formulation of damage accumulation: Δ𝐷 = DMGEXP×𝐷 𝜀𝑓 (1− DMGEXP ) Δ𝜀𝑝 where, 𝐷 𝜀𝑓 Damage value (0 ≤ 𝐷 ≤ 1). For numerical reasons, 𝐷 is initialized to a value of 1.E-20 for all damage types in the first time step Equivalent plastic strain to failure, determined from LCSDG as a function of the current triaxiality value 𝜂 (and Lode parameter 𝐿 as an option). A typical failure curve LCSDG for metal sheet, modelled with shell ele- ments is shown in Figure 2-1 Triaxiality should be monotonically increas- ing in this curve. A reasonable range for triaxiality is -2/3 to 2/3 if shell elements are used (plane stress). For 3-dimensional stress states (solid elements), the possible range of tri- axiality goes from −∞ to +∞, but to get a good resolution in the internal load curve discretization (depending on parameter LCINT of *CON- TROL_SOLUTION) one should define lower limits, e.g. -1 to 1 if LCINT = 100 (default). Δ𝜀𝑝 Equivalent plastic strain increment For constant values of failure strain, this damage rate can be integrated to get a relation of damage and actual equivalent plastic strain: DMGEXP 𝐷 = ( 𝜀𝑝 𝜀𝑓 ) , for 𝜀𝑓 = constant Triaxiality 𝜂 as a measure of the current stress state is defined as 𝜂 = 𝜎𝐻 𝜎𝑀 , with hydrostatic stress 𝜎𝐻 and equivalent von Mises stress 𝜎𝑀. Lode parameter 𝐿 as an additional measure of the current stress state is defined as 𝐿 = 27 𝐽3 𝜎𝑀 3 , with third invariant of the stress deviator 𝐽3. For DMGTYP.EQ.0, damage is accumulated according to the description above, yet no softening and failure is taken into account. Thus, parameters ECRIT, DCRIT and FADEXP will not have any influence. This option can be used to calculate pre-damage in multi-stage deformations without influencing the simulation results. For DMGTYP.EQ.1, elements will be deleted if D ≥ 1. Depending on the set of parameters given by ECRIT (or DCRIT) and FADEXP, a Lemaitre-type coupling of damage and stress (effective stress concept) can be used. Three principal ways of damage definition can be used: 1. Input of a fixed value of critical plastic strain (ECRIT.GT.0.) As soon as the magnitude of plastic strain reaches this value, the current dam- age parameter 𝐷 is stored as critical damage DCRIT and the damage coupling flag is set to unity, in order to facilitate an identification of critical elements in postprocessing. From this point on, damage is coupled to the stress tensor using the following relation: 𝜎 = 𝜎̃ ⎢⎡1 − ( ⎣ 𝐷 − DCRIT 1 − DCRIT FADEXP ) ⎥⎤ ⎦ This leads to a continuous reduction of stress, up to the load-bearing capacity completely vanishing as 𝐷 reaches unity. The fading exponent FADEXP can be defined element size dependent, to allow for the consideration of an element- size dependent amount of energy to be dissipated during element fade-out. 2. Input of a load curve defining critical plastic strain vs. triaxiality (ECRIT < 0.), pointing to load curve ID |ECRIT|. This allows for a definition of triaxiality- dependent material instability, which takes account of that instability and local- ization will occur depending on the actual load case. This offers the possibility to use a transformed Forming Limit Diagram as an input for the expected onset of softening and localization. Using this load curve, the instability measure 𝐹 is accumulated using the following relation, which is similar to the accumulation of damage 𝐷 except for the instability curve is used as an input: Δ𝐹 = DMGEXP 𝜀𝑝,𝑙𝑜𝑐 (1− DMGEXP ) Δ𝜀𝑝 with, 𝐹 Instability measure (0 ≤ 𝐹 ≤ 1). 𝜀p,loc Equivalent plastic strain to instability, determined from ECRIT Δ𝜀𝑝 Equivalent plastic strain increment As soon as the instability measure 𝐹 reaches unity, the current value of damage 𝐷 in the respective element is stored. Damage will from this point on be cou- pled to the flow stress using the relation described above 3. If no input for ECRIT is made, parameter DCRIT will be considered. Coupling of Damage to the stress tensor starts if this value (damage threshold) is exceeded (0 ≤ DCRIT ≤ 1). Coupling of damage to stress is done using the relation described above. This input allows for the use of extreme values also – for example, DCRIT = 1.0 would lead to no coupling at all, and element deletion under full load (brittle fracture). History Variables: History variables of the GISSMO damage model are written to the post-processing database only if NAHSV > 0. As well, NEIPH and NEIPS must be set in *DATABASE_EXTENT_BINARY. The damage history variables start at position ND, which is displayed in d3hsp file, e.g. “first damage history variable = 6” means that ND = 6. For example, if you wish to view the damage parameter (first GISSMO history variable) for a *MAT_024 shell element, you must set NEIPS = 6 and NAHSV = 1. In LS-PrePost, access the damage parameter as history variable #6. *MAT_ADD_EROSION ND Damage parameter 𝐷, (10−20 < 𝐷 ≤ 1 ) ND+1 Damage threshold DCRIT ND+2 Domain flag for damage coupling (0: no coupling, 1: coupling) ND+3 Triaxiality variable 𝜎𝐻/𝜎𝑀 ND+4 Equivalent plastic strain ND+5 Regularization factor for failure strain (determined from LCREGD) ND+6 Exponent for stress fading FADEXP ND+7 Calculated element size ND+8 Instability measure F ND+9 Resultant damage parameter 𝐷 for element size REFSZ ND+10 Resultant damage threshold DCRIT for element size REFSZ ND+11 Averaged triaxiality ND+12 Lode parameter value (only calculated if LCSDG refers to a table) ND+13 Alternative damage value: 𝐷1/DMGEXP ND+14 Averaged Lode parameter DAMAGE INITIATION AND EVOLUTION CRITERIA: As an alternative to GISSMO, the user may invoke up to 5 damage initiation and evolution criteria. For the sake of efficiency, the parameter NCS can be used to only check these criteria in quantified increments of plastic strain. In other words, the criteria are only checked when the effective plastic strain goes beyond NCS, 2 × NCS, 3 × NCS, etc. For NCS = 0 the checks are performed in each step there is plastic flow, a reasonable value of NCS could for instance be NCS = 0.0001. The following theory applies to the DIEM option. Assuming that 𝑛 initiation/evolution types have been specified in the input deck (𝑛 = −IDAM) there is defined at each integration point a damage initiation variable, 𝜔𝐷 𝑖 , and an evolution history variable 𝐷𝑖, such that, and 𝑖 ∈ [0, ∞) 𝜔𝐷 𝐷𝑖 ∈ [0,1], 𝑖 = 1, … 𝑛. These are initially set to zero and evolve with the deformation of the elements according to rules associated with the specific damage initiation and evolution type chosen, see below for details. These quantities can be post-processed as ordinary material history variables and their positions in the history variables array is given in d3hsp, search for the string Damage history listing. The damage initiation variables do not influence the results but serve to indicate the onset of damage. As an alternative, the keyword *DEFINE_MATERIAL_ HISTORIES can be used to output the instability and damage, following *DEFINE_MATERIAL_HISTORIES Properties Label Attributes Description Instability Damage - - - - - - - Maximum initiation variable, 𝑖 max𝑖=1,…,𝑛 𝜔𝐷 - Effective damage 𝐷, see below The damage evolution variables govern the damage in the material and are used to form the global damage 𝐷 ∈ [0,1]. Each criterion is of either of DCTYP set to maximum (DCTYP = 0) or multiplicative (DCTYP = 1), or one could choose to not couple damage to the stress by setting DCTYP = −1. This means that the damage value is calculated and stored, but it is not affecting the stress as for the other options, so if all DCTYP are set to −1 there will be no damage or failure. Letting 𝐼max denote the set of evolution types with DCTYP set to maximum and 𝐼mult denote the set of evolution types with DCTYP set to multiplicative the global damage, 𝐷, is defined as where and, 𝐷 = max(𝐷max, 𝐷mult), 𝐷max = max𝑖∈𝐼max𝐷𝑖 𝐷mult = 1 − ∏ (1 − 𝐷𝑖) . 𝑖∈𝐼mult The damage variable relates the macroscopic (damaged) to microscopic (true) stress by 𝜎 = (1 − 𝐷)𝜎̃ . Once the damage has reached the level of 𝐷erode (=0.99 by default) the stress is set to zero and the integration point is assumed failed and not processed thereafter. For NUMFIP > 0, a shell element is eroded and removed from the finite element model when NUMFIP integration points have failed. For NUMFIP < 0, a shell element is eroded and removed from the finite element model when -NUMFIP percent of the layers have failed. DAMAGE INITIATION, ωD For each evolution type 𝑖, 𝜔𝐷 𝜔𝐷 algorithms for modelling damage initiation. 𝑖 is independent from the evolution of 𝜔𝐷 𝑖 governs the onset of damage. For 𝑖 ≠ 𝑗 the evolution of 𝑗 . The following list enumerates the In this subsection we suppress the superscripted 𝑖 indexing the evolution type. Ductility Based on Stress Triaxiality (DITYP.EQ.0): For the ductile initiation option a function 𝜀𝐷 onset of damage (P1). This is a function of stress triaxiality defined as 𝑝 = 𝜀𝐷 𝑝 (𝜂, 𝜀̇𝑝) represents the plastic strain at 𝜂 = −𝑝/𝑞 with p being the pressure and q the von Mises equivalent stress. Optionally this can be defined as a table with the second dependency being on the effective plastic strain rate 𝜀̇𝑝. The damage initiation history variable evolves according to Shear (DITYP.EQ.1): 𝜀𝑝 𝜔𝐷 = ∫ 𝑑𝜀𝑝 𝜀𝐷 . For the shear initiation option a function 𝜀𝐷 onset of damage (P1). This is a function of a shear stress function defined as 𝑝 (𝜃, 𝜀̇𝑝) represents the plastic strain at 𝑝 = 𝜀𝐷 𝜃 = (𝑞 + 𝑘𝑆𝑝)/𝜏 with p being the pressure, q the von Mises equivalent stress and τ the maximum shear stress defined as a function of the principal stress values 𝜏 = (𝜎major − 𝜎minor)/2. Introduced here is also the pressure influence parameter 𝑘𝑠 (P2). Optionally this can be defined as a table with the second dependency being on the effective plastic strain rate 𝜀̇𝑝. The damage initiation history variable evolves according to 𝜀𝑝 𝜔𝐷 = ∫ 𝑑𝜀𝑝 𝜀𝐷 . *MAT 𝑝 (𝛼, 𝜀̇𝑝) represents the plastic strain at For the MSFLD initiation option a function 𝜀𝐷 onset of damage (P1). This is a function of the ratio of principal plastic strain rates defined as 𝑝 = 𝜀𝐷 𝛼 = 𝜀̇minor 𝜀̇major . The MSFLD criterion is only relevant for shells and the principal strains should be interpreted as the in-plane principal strains. For simplicity the plastic strain evolution in this formula is assumed to stem from an associated von Mises flow rule and whence 𝛼 = 𝑠minor 𝑠major with 𝑠 being the deviatoric stress. This insures that the calculation of 𝛼, is in a sense, robust at the expense of being slightly innacurate for materials with anisotropic yield functions and/or non-associated flow rules. Optionally this can be defined as a table with the second dependency being on the effective plastic strain rate 𝜀̇𝑝. For 𝜀̇𝑝 = 0 the 𝑝 is set to a large number to prevent onset of damage for no plastic evolution. value of 𝜀𝐷 Furthermore, the plastic strain used in this failure criteria is a modified effective plastic strain that only evolves when the pressure is negative, i.e., the material is not affected in compression. This modified plastic strain can be monitored as the second history variable of the initiation history variables in the binary output database. For P3 = 0, the damage initiation history variable is calculated directly from the ratio of (modified) plastic strain and the critical plastic strain 𝜔𝐷 = max𝑡≤𝑇 𝜀𝑝 𝑝 . 𝜀𝐷 This should be interpreted as the maximum value up to this point in time. If P3 = 1 the damage initiation history variable is instead incrementally updated from the ratio of (modified) plastic strain and the critical plastic strain 𝜀𝑝 𝜔𝐷 = ∫ 𝑑𝜀𝑝 𝜀𝐷 . For this initiation option P2 is used to determine the layer in the shell where the criterion is evaluated, if P2 = 0 the criterion is evaluated in the mid-layer only whereas if P2 = 1 it is evaluated in the outer layers only (bottom and top). This can be used to distinguish between a membrane instability typically used for FLD evaluations (P2 = 0), and a bending instability (P2 = 1). As soon as 𝜔𝐷 reaches 1 in any of the integration points of interest, all integration points in the shell goes over in damage mode, i.e., subsequent damage is applied to the entire element. *MAT_ADD_EROSION The FLD initiation criterion is identical to MSFLD with one subtle difference: the plastic strain used for evaluating the criteria is not accounting for the sign of the hydrostatic stress, but is identical to the effective plastic strain directly from the underlying material model. In other words, it is not the modified plastic strain used in the MSFLD criterion, but apart from that it is an identical criterion. Ductile based on normalized principal stress (DITYP.EQ.4): For the ductile initiation option the plastic strain at the onset of damage (P1) is taken as a function of 𝛽 and 𝜀̇𝑝, that is 𝜀𝐷 𝑝 (𝛽, 𝜀̇𝑝), where 𝛽 is the normalized principal stress 𝑝 = 𝜀𝐷 𝛽 = (𝑞 + 𝑘𝑑𝑝)/𝜎major where 𝑝 is the pressure, 𝑞 is the von Mises equivalent stress, 𝜎major is the major principal stress, and where 𝑘𝑑 is the pressure influence parameter specified in the P2 field. Optionally, this can be defined as a table with the second dependency being on the effective plastic strain rate 𝜀̇𝑝. The damage initiation history variable evolves according to 𝜀𝑝 𝜔𝐷 = ∫ 𝑑𝜀𝑝 𝜀𝐷 . DAMAGE EVOLUTION, 𝑫 For the evolution of the associated damage variable D we introduce the plastic displacement 𝑢𝑃 which evolves according to 𝜔𝐷 < 1 𝑢̇𝑝 = { 𝑙𝜀̇𝑝 𝜔𝐷 ≥ 1 with 𝑙 being a characteristic length of the element. Fracture energy is related to plastic displacement as follows 𝑢𝑓 𝐺𝑓 = ∫ 𝜎𝑦𝑑𝑢̇𝑝 where 𝜎𝑦 is the yield stress. The following list enumerates the algorithms available for modelling damage. Linear (DETYP.EQ.0): With this option the damage variable evolves linearly with the plastic displacement 𝑢̇𝑝 𝑝 𝑢𝑓 𝑝 being the plastic displacement at failure (Q1). If Q1 is negative, then –Q1 refers 𝑝(𝜂, 𝐷), and 𝑝 as a function of triaxiality and damage, i.e., 𝑢𝑓 with 𝑢𝑓 to a table that defines 𝑢𝑓 importantly the damage evolution law is changed generalized to 𝑝 = 𝑢𝑓 𝐷̇ = 𝐷̇ = 𝑢̇𝑝 ∂𝑢𝑓 ∂𝐷 Linear (DETYP.EQ.1): With this option the damage variable evolves linearly as follows 𝐷̇ = 𝑢̇𝑝 𝑝 𝑢𝑓 where 𝑢𝑓 𝑝 = 2𝐺𝑓 /𝜎𝑦0 𝑢𝑓 𝑝 and 𝜎𝑦0 is the yield stress when failure criterion is reached. *MAT_ADD_FATIGUE The ADD_FATIGUE option defines the S-N fatigue property of a material model. Card 1 1 2 3 Variable MID LCID LTYPE Type I I Default none -1 I 0 4 A F 5 B F F I 0 I 0 0.0 0.0 none 6 7 8 STHRES SNLIMT SNTYPE S-N Curve Segment Cards. Include one card for each additional S-N curve segment. Between zero and seven of these cards may be included in the deck. This input ends at the next keyword (“*”) card. Card 2 1 2 3 Variable Type Default 4 Ai F 5 Bi F 6 7 8 STHRESi F 0.0 0.0 none VARIABLE DESCRIPTION MID LCID Material identification for which the fatigue property applies. S-N fatigue curve ID. GT.0: S-N fatigue curve ID EQ.-1: S-N fatigue curve uses equation 𝑁𝑆𝑏 = 𝑎 EQ.-2: S-N fatigue curve uses equation log(𝑆) = 𝑎 − 𝑏 log(𝑁) EQ.-3: S-N fatigue curve uses equation 𝑆 = 𝑎 𝑁𝑏 LTYPE Type of S-N curve. EQ.0: Semi-log interpolation (default) EQ.1: Log-Log interpolation EQ.2: Linear-Linear interpolation VARIABLE DESCRIPTION A B STHRES SNLIMT Material parameter 𝑎 in S-N fatigue equation. Material parameter 𝑏 in S-N fatigue equation. Fatigue threshold stress if the S-N curve is defined by equation (LCID < 0). If LCID > 0 SNLIMNT determines the algorithm used when stress is lower than the lowest stress on S-N curve. EQ.0: use the life at the last point on S-N curve EQ.1: extrapolation from the last two points on S-N curve EQ.2: infinity. If LCID < 0 SNLIMIT determines the algorithm used when stress is lower than STHRES. EQ.0: use the life at STHRES EQ.1: Ignored. only applicable for LCID > 0 EQ.2: infinity. SNTYPE Stress type of S-N curve. EQ.0: stress range (default) EQ.1: stress amplitude. Ai Bi Material parameter 𝑎 in S-N fatigue equation for the i-th segment. Material parameter 𝑏 in S-N fatigue equation for the i-th segment. STHRESi Fatigue threshold stress for the i-th segment. Remarks: 1. S-N curves can be defined by *DEFINE_CURVE, or for LCID < 0 by when LCID = -1 or for LCID = -2 log(𝑆) = 𝑎 − 𝑏 log(𝑁) 𝑁𝑆𝑏 = 𝑎 or for LCID = -3 𝑆 STHRES2 STHRES1 𝑁𝑆𝑏2 = 𝑎2 𝑁𝑆𝑏1 = 𝑎1 𝑁 Figure 2-2. S-N Curve having multiple slopes 𝑆 = 𝑎 𝑁𝑏 where 𝑁 is the number of cycles for fatigue failure and 𝑆 is the stress amplitude. Note that the two equations can be converted to each other, with some minor algebraic manipulation on the constants 𝑎 and 𝑏. To define S-N curve with multiple slopes, the S-N curve can be split into multi- ple segments and each segment is defined by a set of parameters Ai, Bi and STHRESi. Up to 8 sets of the parameters (Ai, Bi and STHRESi) can be defined. The lower limit of the i-th segment is represented by the threshold stress STHRESi, as shown in Figure 2-2. This only applies to the case where the S-N curve is defined by equations (LCID = -1 or LCID = -2) 2. This model is applicable to frequency domain fatigue analysis, defined by the keywords: *FREQUENCY_DOMAIN_RANDOM_VIBRATION_FATIGUE, and *FREQUENCY_DOMAIN_SSD_FATIGUE . *MAT_ADD_GENERALIZED_DAMAGE This option provides a way of including generalized (tensor type) damage and failure in standard LS-DYNA material models. The basic idea is to apply a general damage model (e.g. GISSMO) using several history variables as damage driving quantities at the same time. With that feature it may be possible to obtain e.g. anisotropic damage behavior or separate stress degradation for volumetric and deviatoric deformations. A maximum of three simultaneous damage evolutions (i.e. definition of 3 history variables) is possible. A detailed description of this model can be found in Erhart et al. [2017]. This option currently applies to shell element types 1, 2, 3, 4, 16, and 17 and solid element types -2, -1, 1, 2, 3, 4, 10, 13, 15, 16, and 17. Card 1 1 2 3 4 5 6 7 8 Variable MID IDAM DTYP REFSZ NUMFIP PDDT NHIS Type I Default none Card 2 1 I 0 2 I 0 3 F F 0.0 1.0 4 5 6 I 0 7 I 1 8 Variable HIS1 HIS2 HIS3 IFLG1 IFLG2 IFLG3 Type Default I 0 I I none none Card 3 1 2 3 I 0 4 I 0 5 I 0 6 Variable D11 D22 D33 D44 D55 D66 Type I I I I I I Default none none none none none none 7 (shells) *MAT_ADD_GENERALIZED_DAMAGE 1 2 3 4 5 6 7 8 Variable D12 D21 D24 D42 D14 D41 Type I I I I I I Default none none none none none none Card 4 (solids) 1 2 3 4 5 6 7 8 Variable D12 D21 D23 D32 D13 D31 Type I I I I I I Default none none none none none none Damage definition cards for IDAM = 1 (GISSMO). 2 x NHIS cards have to be defined, i.e. two cards for each history variable. First Card for history variable HISn: Card 5… 1 2 3 4 5 6 7 8 Variable LCSDG ECRIT DMGEXP DCRIT FADEXP LCREG Type Default I 0 F F F F 0.0 1.0 0.0 1.0 I Second Card for history variable HISn: Card 6… 1 2 3 4 5 6 7 8 Variable LCSRS SHRF BIAXF LCDLIM Type Default I 0 F F 0.0 0.0 I 0 VARIABLE DESCRIPTION MID Material ID for which this generalized damage definition applies. IDAM Flag for damage model. EQ.0: no damage model is used. EQ.1: GISSMO damage model. DTYP Flag for damage behavior. EQ.0: Damage is accumulated, no coupling to flow stress, no failure. EQ.1: Damage is accumulated, element failure occurs for D = 1. REFSZ Reference element size, for which an additional output of damage will be generated. This is necessary to ensure the applicability of resulting damage quantities when transferred to different mesh sizes. NUMFIP Number of failed integration points prior to element deletion. The default is unity. LT.0: |NUMFIP| is the percentage of layers which must fail before element fails. PDDT NHIS HISn *MAT_ADD_GENERALIZED_DAMAGE DESCRIPTION Pre-defined damage tensors. If non-zero, damage tensor coefficients D11 to D66 on cards 3 and 4 will be ignored. See remarks for details. EQ.0: No pre-defined damage tensor is used. EQ.1: Isotropic damage tensor. EQ.2: 2-parameter isotropic damage tensor for volumetric- deviatoric split. EQ.3: Anisotropic damage tensor as in MAT_104 (FLAG = - 1). EQ.4: 3-parameter damage tensor associated with IFLG1 = 2. Number of history variables as driving quantities (min = 1, max = 3). Choice of variable as driving quantity for damage, called “history value” in the following. EQ.0: Equivalent plastic strain rate is the driving quantity for the damage if IFLG1 = 0. Alternatively if IFLG1 = 1, components of the plastic strain rate tensor are driving quantities for damage . GT.0: The rate of the additional history variable HISn is the driving quantity for damage. IFLG1 should be set to 0. LT.0: the damage *DEFINE_FUNCTION driving quantities as a function of the components of the plastic strain rate tensor, IFLG1 should be set to 1. IDs defining IFLG1 Damage driving quantities EQ.0: Rates of history variables HISn. EQ.1: Specific components of the plastic strain rate tensor, see remarks for details. EQ.2: Predefined functions of plastic strain rate components for orthotropic damage model, HISn inputs will be ig- nored, IFLG2 should be set to 1. This option is for shell elements only. VARIABLE DESCRIPTION IFLG2 Damage strain coordinate system EQ.0: Local element system (shells) or global system (solids). EQ.1: Material system, only applicable for non-isotropic material models. Supported models for shells: all mate- rials with AOPT feature. Supported models for solids: 22, 33, 41-50, 103, 122, 157, 233. EQ.2: Principal strain system (rotating). EQ.3: Principal strain system (fixed when instabil- ity/coupling starts). IFLG3 Erosion criteria and damage coupling system EQ.0: Erosion occurs when one of the damage parameters computed reaches unity, the damage tensor compo- nents are based on the individual damage parameters d1 to d3. EQ.1: Erosion occurs when a single damage parameter D reaches unity, the damage tensor components are based on this single damage parameter. D11…D31 LCSDG DEFINE_FUNCTION IDs for damage tensor coefficients, see remarks. Load curve ID defining corresponding history value to failure vs. triaxiality. ECRIT Critical history value (material instability), see below. LT.0.0: |ECRIT| is load curve ID defining critical history value vs. triaxiality. EQ.0.0: Fixed value DCRIT defining critical damage is read. GT.0.0: Fixed value for stress-state independent critical history value. DMGEXP Exponent for nonlinear damage accumulation. DCRIT Damage threshold value (critical damage). If a Load curve of critical history value or fixed value is given by ECRIT, input is ignored. *MAT_ADD_GENERALIZED_DAMAGE DESCRIPTION FADEXP Exponent for damage-related stress fadeout. LT.0.0: |FADEXP| is load curve ID defining element-size dependent fading exponent. GT.0.0: Constant fading exponent. LCREG LCSRS Load curve ID defining element size dependent regularization factors for history value to failure. Load curve ID defining failure history value scaling factor for LCSDG vs. history value rate. If the first rate value in the curve is negative, it is assumed that all rate values are given as natural logarithm of the history rate. GT.0: scale ECRIT, too LT.0: do not scale ECRIT. SHRF Reduction factors for regularization at triaxiality = 0 (shear) BIAXF Reduction factors for regularization at triaxiality = 2/3 (biaxial) Load curve ID defining damage limit values as a function of triaxiality. Damage can be restricted to values less than 1.0 to for certain prevent triaxialities. further stress reduction and failure LCDLIM Remarks: The GISSMO damage model is described in detail in the remarks of *MAT_ADD_ERO- SION. If NHIS = 1 and HIS1 = 0 is used, this new feature (“MAGD”) behaves just the same as before (“GISSMO”). The main difference with this new keyword is that up to 3 independent but simultaneous damage evolutions are possible. Therefore, parameters LCSDG, ECRIT, DMGEXP, DCRIT, FADEXP, LCREGD, LCSRS, SHRF, BIAXF, and LCDLIM can be defined separately for each history variable. The relation between nominal (damaged) stresses 𝜎𝑖𝑗 and effective (undamaged) stresses 𝜎̃𝑖𝑗 is now expressed as 𝜎11 ⎤ ⎡ 𝜎22 ⎥ ⎢ 𝜎33 ⎥ ⎢ ⎥ ⎢ 𝜎12 ⎥ ⎢ ⎥ ⎢ 𝜎23 𝜎31⎦ ⎣ = 𝐷11 𝐷12 𝐷13 ⎡ 𝐷21 𝐷22 𝐷23 ⎢ ⎢ 𝐷31 𝐷32 𝐷33 ⎢ ⎢ ⎢ ⎢ ⎣ 0 𝐷44 𝐷55 ⎤ ⎥ ⎥ ⎥ ⎥ ⎥ ⎥ 𝐷66⎦ 𝜎̃11 ⎤ ⎡ 𝜎̃22 ⎥ ⎢ ⎥ ⎢ 𝜎̃33 ⎥ ⎢ ⎥ ⎢ 𝜎̃12 ⎥ ⎢ 𝜎̃23 ⎥ ⎢ 𝜎̃31⎦ ⎣ with damage tensor 𝐷. Each damage tensor coefficient 𝐷𝑖𝑗 can be defined via *DE- FINE_FUNCTION as a function of damage parameters 𝑑1 to 𝑑3. For simple isotropic damage driven by plastic strain (NHIS = 1, HIS1 = 0, IFLG1 = IFLG2 = IFLG3 = 0) that would be 𝜎11 ⎤ ⎡ 𝜎22 ⎥ ⎢ 𝜎33 ⎥ ⎢ ⎥ ⎢ 𝜎12 ⎥ ⎢ ⎥ ⎢ 𝜎23 𝜎31⎦ ⎣ = (1 − 𝑑1) ⎡ ⎢ ⎢ ⎢ ⎢ ⎢ ⎣ ⎤ ⎥ ⎥ ⎥ ⎥ ⎥ 1⎦ 𝜎̃11 ⎤ ⎡ 𝜎̃22 ⎥ ⎢ ⎥ ⎢ 𝜎̃33 ⎥ ⎢ ⎥ ⎢ 𝜎̃12 ⎥ ⎢ 𝜎̃23 ⎥ ⎢ 𝜎̃31⎦ ⎣ That means the following function should be defined for D11 to D66 (Card 3): *DEFINE_FUNCTION 1,D11toD66 func1(d1,d2,d3)=(1.0-d1) and all entries in Card 4 can be left empty or equal zero in that case. If GISSMO (IDAM = 1) is used, the damage parameters used in those functions are internally replaced by 𝑑𝑖 → ( 𝑑𝑖 − 𝐷𝐶𝑅𝐼𝑇𝑖 1 − 𝐷𝐶𝑅𝐼𝑇𝑖 𝐹𝐴𝐷𝐸𝑋𝑃𝑖 ) In the case of plane stress (shell) elements, coupling between normal stresses and shear stresses is implemented and the damage tensor is defined as below : 𝜎11 ⎤ ⎡ 𝜎22 ⎥ ⎢ ⎥ ⎢ ⎥ ⎢ 𝜎12 ⎥ ⎢ ⎥ ⎢ 𝜎23 𝜎31⎦ ⎣ = 𝐷11 𝐷12 ⎡ 𝐷21 𝐷22 ⎢ ⎢ ⎢ ⎢ 𝐷41 𝐷42 ⎢ ⎢ ⎣ 0 𝐷14 0 𝐷24 𝐷33 0 𝐷44 𝐷55 ⎤ ⎥ ⎥ ⎥ ⎥ ⎥ ⎥ 𝐷66⎦ 𝜎̃11 ⎤ ⎡ 𝜎̃22 ⎥ ⎢ ⎥ ⎢ ⎥ ⎢ 𝜎̃12 ⎥ ⎢ 𝜎̃23 ⎥ ⎢ 𝜎̃31⎦ ⎣ Since the evaluation of *DEFINE_FUNCTION for variables D11 to D66 is relatively time consuming, pre-defined damage tensors (PDDT) can be used. Currently the following options are available for shell elements: PDDT = 1 (1 − 𝐷1) ⎡ ⎢ ⎢ ⎢ ⎢ ⎢ ⎣ ⎤ ⎥ ⎥ ⎥ ⎥ ⎥ 1⎦ PDDT = 3 PDDT = 4 *MAT_ADD_GENERALIZED_DAMAGE 𝐷1 − 1 𝐷2 𝐷2 ⎡1 − 2 ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎣ 𝐷1 − 1 𝐷2 𝐷1 − 1 1 − 2 𝐷2 𝐷1 − 1 1 − 𝐷1 ⎤ ⎥ ⎥ ⎥ ⎥ ⎥ ⎥ ⎥ 1⎦ 1 − 𝐷1 ⎡ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎣ 1 − 𝐷2 1 − 1 (𝐷1 + 𝐷2) 1 − 1 𝐷2 ⎤ ⎥ ⎥ ⎥ ⎥ ⎥ ⎥ ⎥ 1 − 1 𝐷1⎦ 1 − 𝐷1 ⎡ ⎢ ⎢ ⎢ ⎢ ⎢ ⎣ 1 − 𝐷2 1 − 𝐷3 ⎤ ⎥ ⎥ ⎥ ⎥ ⎥ 1⎦ and the following ones for solid elements: PDDT = 1 PDDT = 2 𝐷1 − 1 𝐷2 𝐷2 𝐷2 ⎡1 − 2 ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎣ 𝐷1 − 1 𝐷1 − 1 (1 − 𝐷1) ⎡ ⎢ ⎢ ⎢ ⎢ ⎢ ⎣ ⎤ ⎥ ⎥ ⎥ ⎥ ⎥ 1⎦ 𝐷1 − 1 1 − 2 𝐷2 𝐷1 − 1 𝐷2 𝐷2 𝐷1 − 1 1 − 2 𝐷1 − 1 𝐷1 − 1 𝐷2 𝐷2 𝐷1 − 1 𝐷2 1 − 𝐷1 1 − 𝐷1 ⎤ ⎥ ⎥ ⎥ ⎥ ⎥ ⎥ ⎥ ⎥ 1 − 𝐷1⎦ 3 1 − 𝐷1 ⎡ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎣ 1 − 𝐷2 1 − 𝐷3 1 − 1 (𝐷1 + 𝐷2) *MAT ⎤ 1 − 1 (𝐷2 + 𝐷3) 1 − 1 (𝐷3 + 𝐷1)⎦ History Variables: The increment of the damage parameter is computed in GISSMO based on a driving quantity that has the dimension of a strain rate : ˙ 𝑑˙ = 𝑛𝑑1−1 𝑛⁄ 𝐻𝐼𝑆𝚤 𝑒𝑝𝑓 The history variables defined by the user through HISi should thus have the dimension of a strain as the rate is computed internally by MAT_ADD_GENERALIZED_DAM- AGE: HISı̇ = HISi(𝑡𝑛+1) − HISi(𝑡𝑛) 𝑡𝑛+1 − 𝑡𝑛 History variables can either come directly from associated material models (IFLG1 = 0 and HISi > 0), or they can be equivalent to plastic strain rate tensor components (IFLG1 = 1 and HISi = 0): HIṠ 1 = 𝜀̇𝑥𝑥 𝑝 , HIṠ 2 = 𝜀̇𝑥𝑥 𝑝 , HIṠ 3 = 𝜀̇𝑥𝑦 𝑝 (IFLG2 = 0) HIṠ 1 = 𝜀̇𝑎𝑎 𝑝 , HIṠ 2 = 𝜀̇𝑏𝑏 𝑝, HIṠ 2 = 𝜀̇2 𝑝 (IFLG2 = 1) 𝑝 , HIṠ 3 = 𝜀̇𝑎𝑏 𝑝, HIṠ 3 = 0 (IFLG2 = 2) HIṠ 1 = 𝜀̇1 or they can be provided via *DEFINE_FUNCTIONs by the user (IFLG1 = 1 and HISi < 0): HIṠ 𝑖 = 𝑓𝑖(𝜀̇𝑥𝑥 𝑝 , 𝜀̇𝑦𝑦 𝑝 , 𝜀̇𝑧𝑧 𝑝 , 𝜀̇𝑥𝑦 𝑝 , 𝜀̇𝑦𝑧 𝑝 , 𝜀̇𝑧𝑥 𝑝 ) (IFLG2 = 0) HIṠ 𝑖 = 𝑓𝑖(𝜀̇𝑎𝑎 𝑝 , 𝜀̇𝑏𝑏 𝑝 , 𝜀̇𝑧𝑧 𝑝 , 𝜀̇𝑎𝑏 𝑝 , 𝜀̇𝑏𝑧 𝑝 , 𝜀̇𝑧𝑎 𝑝 ) (IFLG2 = 1) HIṠ 𝑖 = 𝑓𝑖(𝜀̇1 𝑝, 𝜀̇2 𝑝) (IFLG2 = 2) e.g. the following example defines a history variable (HISi = -1234) as function of the transverse shear strains in material coordinate system a-b-z for shells: *DEFINE_FUNCTION 1234 fhis1(eaa,ebb,ezz,eab,ebz,eza)=1.1547*sqrt(ebz**2+eza**2) The plastic strain rate tensor is not always available in the material law and is estimated as: 𝛆̇𝑝 = 𝜀̇𝑒𝑓𝑓 𝜀̇𝑒𝑓𝑓 [𝛆̇ − 𝜀̇𝒗𝒐𝒍 𝛅] This is a good approximation for isochoric materials with small elastic strains (e.g. metals) and correct for J2 plasticity. The following table gives an overview of the driving quantities used for incrementing the damage in function of the input parameters (strain superscript “p” for “plastic” is omitted for convenience): IFLG1 IFLG2 HISi > 0 HISi = 0 HISi < 0 0 0 0 1 1 1 2 2 2 0 1 2 0 1 2 0 1 2 ˙ HISı ˙ HISı ˙ HISı N/A N/A N/A 𝜀˙ N/A N/A 𝜀˙𝑖𝑗 𝑚𝑎𝑡 𝜀˙𝑖𝑗 𝜀˙𝑖 N/A N/A N/A 𝑓 (𝜀˙𝑖𝑗) 𝑓 (𝜀˙𝑖𝑗 𝑚𝑎𝑡) 𝑓 (𝜀˙𝑖) N/A Preprogrammed functions of plastic strain rate N/A Postprocessing History Variables: History variables of the GENERALIZED_DAMAGE model are written to the post- processing database behind those already occupied by the material model which is used in combination: Variable Description ND Triaxiality variable 𝜎𝐻/𝜎𝑀 ND+1 Lode parameter value ND+2 Single damage parameter 𝐷, (10−20 < 𝐷 ≤ 1 ), only for IFLG3 = 1 ND+3 Damage parameter 𝑑1 ND+4 Damage parameter 𝑑2 ND+5 Damage parameter 𝑑3 ND+6 Damage threshold DCRIT1 ND+7 Damage threshold DCRIT2 ND+8 Damage threshold DCRIT3 ND+12 History variable HIS1 ND+13 History variable HIS2 ND+14 History variable HIS3 ND+15 Angle between principal and material axes ND+21 Characteristic element size (used in LCREG) For instance, ND = 6 for *MAT_024, ND = 9 for *MAT_036, or ND = 23 for *MAT_187. Exact information of the variable locations can be found in the d3hsp section “MAGD damage history listing”. For consolidation calculations. *MAT_ADD_PERMEABILITY Card 1 1 2 3 4 5 6 7 8 Variable MID PERM (blank) (blank) THEXP LCKZ Type I F F I Default none none 0.0 none VARIABLE DESCRIPTION MID Material identification – must be same as the structural material. PERM Permeability THEXP Undrained volumetric thermal expansion coefficient (Units: 1/temperature). If negative, then –THEXP is the ID of a loadcurve giving thermal expansion coefficient (y-axis) versus temperature (x-axis). LCKZ Loadcurve giving factor on PERM versus z-coordinate. (X-axis – z-coordinate, yaxis – non dimensional factor) Remarks: The units of PERM are length/time (volume flow rate of water per unit area per gradient of pore pressure head). THEXP represents the thermal expansion of the material caused by the pore fluid. It should be set equal to nαw, where n is the porosity of the soil and αw is the volumetric thermal expansion coefficient of the pore fluid. If the pore fluid is water, the thermal expansion coefficient varies strongly with temperature; a curve of coefficient versus temperature may be input instead of a constant value. See notes under *CONTROL_PORE_FLUID For pore air pressure calculations. *MAT Card 1 1 2 3 4 5 6 7 8 Variable MID PA_RHO PA_PRE PORE Type I I F F Default none AIR_RO AIR_RO 1. Remarks 1 1, 2 Card 2 1 2 3 4 5 6 7 8 Variable PERM1 PERM2 PERM3 CDARCY CDF LCPGD1 LCPGD2 LCPGD3 Type F F F F F I I I Default 0. PERM1 PERM1 1. 0. none LCPGD1 LCPGD1 Remarks 2, 3, 4, 5 2, 3, 4, 5 2, 3, 4, 5 1 1, 5 6 6 6 VARIABLE DESCRIPTION MID Material identification – must be same as the structural material. PA_RHO PA_PRE Initial density of pore air, default to atmospheric air density, AIR_RO, defined in *CONTROL_PORE_AIR Initial pressure of pore air, default to atmospheric air pressure, AIR_P, defined in *CONTROL_PORE_AIR PORE Porosity, ratio of pores to total volume, default to 1. PERM[1-3] Permeability of pore air along 𝑥, 𝑦 and 𝑧-direction. If less than 0 – PERM[1-3] is taken to be the curve ID defining the permeability coefficient as a function of volume ratio of current volume to volume in the stress free state. *MAT_ADD_PORE_AIR DESCRIPTION CDARCY Coefficient of Darcy’s law CDF Coefficient of Dupuit-Forchheimer law LCPGD1~3 Curves defining non-linear Darcy’s laws along x, y and z- directions, see Remarks 6. Remarks: 1. Card 1. This card must be defined for all materials requiring consideration of pore air pressure. The pressure contribution of pore air is (𝜌 − 𝜌atm)RT× PORE, where 𝜌 and 𝜌atm are the current and atmospheric air density, 𝑅 is air’s gas constant, 𝑇 is atmospheric air temperature and PORE is the porosity. The values for 𝑅, 𝑇 and PORE are assumed to be constant during simulation. 2. Permeability Model. The unit of PERMi is [Length]3[time]/[mass], (air flow velocity per gradient of excess pore pressure), i.e. (CDARCY + CDF × |𝑣𝑖|) × PORE × 𝑣𝑖 = PERM𝑖 × 𝜕𝑃𝑎 𝜕𝑥𝑖 , 𝑖 = 1,2,3 where 𝑣i is the pore air flow velocity along the ith direction, 𝜕𝑃𝑎/𝜕𝑥𝑖 is the pore air pressure gradient along the ith direction, and 𝑥1 = 𝑥, 𝑥2 = 𝑦, 𝑥3 = 𝑧. 3. Default Values for PERM2 and PERM3. PERM2 and PERM3 are assumed to be equal to PERM1 when they are not defined. A definition of “0” means no permeability. 4. Local Coordinate Systems. (x,y,z), or (1,2,3), refers to the local material coordinate system (a,b,c) when MID is an orthotropic material, such as *MAT_- 002 or *MAT_142; otherwise it refers to the global coordinate system. 5. CDF for Viscosity. CDF can be used to consider the viscosity effect for high speed air flow 6. Nonlinearity. LCPGDi can be used to define a non-linear Darcy’s law as follows: (CDARCY + CDF × |𝑣𝑖|) × PORE × 𝑣𝑖 = PERM𝑖 × 𝑓𝑖 𝜕𝑃𝑎 𝜕𝑥𝑖 , 𝑖 = 1,2,3 where 𝑓𝑖 is value of the function defined by the LCPGDi field. The linear ver- siono Darcy’s law of Remark 2, can be recovered when the LCPGDi curves are defined as straight lines of slope of 1. *MAT The ADD_THERMAL_EXPANSION option is used to occupy an arbitrary material model in LS-DYNA with a thermal expansion property. This option applies to all nonlinear solid, shell, thick shell and beam elements and all material models except those models which use resultant formulations such as *MAT_RESULTANT_PLASTIC- ITY and Orthotropic expansion effects are supported for anisotropic materials. *MAT_SPECIAL_ORTHOTROPIC. Card 1 1 2 3 4 5 6 7 8 Variable PID LCID MULT LCIDY MULTY LCIDZ MULTZ Type I I F I F I F Default none none 1.0 LCID MULT LCID MULT VARIABLE DESCRIPTION PID LCID MULT LCIDY Part ID for which the thermal expansion property applies For isotropic material models, LCIDY, MULTY, LCIDZ, and MULTZ are ignored, and LCID is the load curve ID defining the thermal expansion coefficient as a function of temperature. If zero, the thermal expansion coefficient is constant and equal to MULT. For anisotropic material models, LCID and MULT define the thermal expansion coefficient in the local material a-direction. Scale factor scaling load curve given by LCID. Load curve ID defining the thermal expansion coefficient in local material b-direction as a function of temperature. If zero, the thermal expansion coefficient in the local material b-direction is constant and equal to MULTY. If MULTY = 0 as well, LCID and MULT define the thermal expansion coefficient in the local material b-direction. MULTY Scale factor scaling load curve given by LCIDY. LCIDZ *MAT_ADD_THERMAL_EXPANSION DESCRIPTION Load curve ID defining the thermal expansion coefficient in local material c-direction as a function of temperature. If zero, the thermal expansion coefficient in the local material c-direction is constant and equal to MULTZ. If MULTZ = 0 as well, LCID and MULT define the thermal expansion coefficient in the local material c-direction. MULTZ Scale factor scaling load curve given by LCIDZ. Remarks: When invoking the isotropic thermal expansion property (no use of the local y and z parameters) for a material, the stress update is based on the elastic strain rates given by 𝑒 = 𝜀̇𝑖𝑗 − 𝛼(𝑇)𝑇̇𝛿𝑖𝑗 𝜀̇𝑖𝑗 rather than on the total strain rates 𝜀̇𝑖𝑗. For a material with the stress based on the deformation gradient 𝐹𝑖𝑗, the elastic part of the deformation gradient is used for the stress computations 𝑒 = 𝐽𝑇 𝐹𝑖𝑗 −1/3𝐹𝑖𝑗 where 𝐽𝑇 is the thermal Jacobian. The thermal Jacobian is updated using the rate given by 𝐽 ̇𝑇 = 3𝛼(𝑇)𝑇̇𝐽𝑇. For orthotropic properties, which apply only to materials with anisotropy, these equations are generalized to and where the 𝛽𝑖 are updated as 𝑒 = 𝜀̇𝑖𝑗 − 𝛼𝑘(𝑇)𝑇̇𝑞𝑖𝑘𝑞𝑗𝑘 𝜀̇𝑖𝑗 𝑒 = 𝐹𝑖𝑘𝛽𝑙 𝐹𝑖𝑗 −1𝑄𝑘𝑙𝑄𝑗𝑙 𝛽̇ 𝑖 = 𝛼𝑖(𝑇)𝑇̇𝛽𝑖. Here 𝑞𝑖𝑗 represents the matrix with material directions with respect to the current configuration whereas 𝑄𝑖𝑗 are the corresponding directions with respect to the initial configuration. For (shell) materials with multiple layers of different anisotropy directions, the mid surface layer determines the orthotropy for the thermal expansion. *MAT In nonlocal failure theories, the failure criterion depends on the state of the material within a radius of influence which surrounds the integration point. An advantage of nonlocal failure is that mesh size sensitivity on failure is greatly reduced leading to results which converge to a unique solution as the mesh is refined. Without a nonlocal criterion, strains will tend to localize randomly with mesh refinement leading to results which can change significantly from mesh to mesh. The nonlocal failure treatment can be a great help in predicting the onset and the evolution of material failure. This option can be used with two and three-dimensional solid elements, and three-dimensional shell elements and thick shell elements. This option applies to a subset of elastoplastic materials that include a damage-based failure criterion. Card 1 1 2 Variable IDNL PID Type I I 3 P F 4 Q F 5 L F 6 7 8 NFREQ NHV I I Default none none none none none none none History Cards. Include as many cards as needed to set NHV variables. One card 2 will be read even if NHV = 0. Card 2 1 2 3 4 5 6 7 8 Variable NL1 NL2 NL3 NL4 NL5 NL6 NL7 NL8 Type I I I I I I I I Default none none none none none none none none Symmetry Plane Cards. Define one card for each symmetry plane. Up to six symmetry planes can be defined. The next “*” card terminates this input. Cards 3 1 2 3 4 5 6 7 8 Variable XC1 YC1 ZC1 XC2 YC2 ZC2 Type F F F F F F Default none none none none none none VARIABLE DESCRIPTION IDNL PID Nonlocal material input ID. Part ID for nonlocal material. P Q L NFREQ Exponent of weighting function. A typical value might be 8 depending somewhat on the choice of L. See equations below. Exponent of weighting function. A typical value might be 2. See equations below. Characteristic length. This length should span a few elements. See equations below. Number of time steps between searching for integration points that lie in the neighborhood. Nonlocal smoothing will be done each cycle using these neighbors until the next search is done. The neighbor search can add significant computational time so it is suggested that NFREQ be set to value of 10 to 100 depending on the problem. This parameter may be somewhat problem dependent. If NFREQ = 0, a single search will be done at the start of the calculation. NHV Define the number of history variables for nonlocal treatment. NL1, …, NL8 Identifies the history variable(s) for nonlocal treatment. Define NHV values (maximum of 8 values per line). XC1, YC1, ZC1 Coordinate of point on symmetry plane. XC2, YC2, ZC2 Coordinate of a point along the normal vector. *MAT For elastoplastic material models in LS-DYNA which use the plastic strain as a failure criterion, setting the variable NL1 to 1 would tag plastic strain for nonlocal treatment. A sampling of other history variables that can be tagged for nonlocal treatment are listed in the table below. The value in the third column in the table below corresponds to the history variable number as tabulated at http://www.dynasupport.com/howtos- /material/history-variables. Note that the NLn value is the history variable number plus 1. Material Model Name JOHNSON_COOK PLASTICITY_WITH_DAMAGE DAMAGE_1 DAMAGE_2 JOHNSON_HOLMQUIST_CONCRETE GURSON 15 81 104 105 111 120 *MAT_NONLOCAL NLn Value History Variable Number 5 (shells); 7 (solids) 4 (shells); 6 (solids) 2 4 2 2 2 1 3 1 1 1 In applying the nonlocal equations to shell and thick shell elements, integration points lying in the same plane within the radius determined by the characteristic length are considered. Therefore, it is important to define the connectivity of the shell elements consistently within the part ID, e.g., so that the outer integration points lie on the same surface. The equations and our implementation are based on the implementation by Worswick and Lalbin [1999] of the nonlocal theory to Pijaudier-Cabot and Bazant [1987]. Let Ω𝑟 be the neighborhood of radius, L, of element 𝑒𝑟 and {𝑒𝑖}𝑖=1,...,𝑁𝑟 the list of elements included in Ω𝑟, then 𝑟 = 𝑓 ̇(𝑥𝑟) = 𝑓 ̇ 𝑊𝑟 local𝑤(𝑥𝑟 − 𝑦) ∫ 𝑓 ̇ 𝛺𝑟 𝑑𝑦 ≈ 𝑊𝑟 𝑁𝑟 ∑ 𝑓 ̇ 𝑖=1 local 𝑤𝑟𝑖 𝑉𝑖 where 𝑊𝑟 = 𝑊(𝑥𝑟) = ∫ 𝑤(𝑥𝑟 − 𝑦) 𝑑𝑦 ≈ ∑ 𝑤𝑟𝑖𝑉𝑖 𝑁𝑟 𝑤𝑟𝑖 = 𝑤(𝑥𝑟 − 𝑦𝑖) = 𝑖=1 [1 + ( ∥𝑥𝑟 − 𝑦𝑖∥ 𝑞 ) ] Figure 2-3. Here 𝑓 ̇ 𝑟 and 𝑥𝑟 are respectively the nonlocal rate of increase of damage and the center of the element 𝑒𝑟, and 𝑓 ̇ , 𝑉𝑖 and 𝑦𝑖 are respectively local the local rate of increase of damage, the volume and the center of element 𝑒𝑖. *MAT_001 This is Material Type 1. This is an isotropic hypoelastic material and is available for beam, shell, and solid elements in LS-DYNA. A specialization of this material allows the modeling of fluids. Available options include: <BLANK> FLUID such that the keyword cards appear: *MAT_ELASTIC or MAT_001 *MAT_ELASTIC_FLUID or MAT_001_FLUID The fluid option is valid for solid elements only. Card 1 1 Variable MID 2 RO Type A8 F 3 E F 4 PR F 5 DA F 6 DB F 7 K F 8 Default none none none 0.0 0.0 0.0 0.0 Additional card for FLUID keyword option. 3 4 5 6 7 8 Card 2 Variable 1 VC Type F 2 CP F Default none 1.0E+20 VARIABLE MID LS-DYNA R10.0 DESCRIPTION Material identification. A unique number or label not exceeding 8 *MAT_ELASTIC DESCRIPTION Mass density. Young’s modulus. Poisson’s ratio. Axial damping factor (used for Belytschko-Schwer beam, type 2, only). Bending damping factor (used for Belytschko-Schwer beam, type 2, only). Bulk Modulus (define for fluid option only). Tensor viscosity coefficient, values between .1 and .5 should be okay. Cavitation pressure (default = 1.0e+20). RO E PR DA DB K VC CP Remarks: This hypoelastic material model may not be stable for finite (large) strains. If large strains are expected, a hyperelastic material model, e.g., *MAT_002, would be more appropriate. The axial and bending damping factors are used to damp down numerical noise. The update of the force resultants, 𝐹𝑖, and moment resultants, 𝑀𝑖, includes the damping factors: 𝑛+1 = 𝐹𝑖 𝐹𝑖 𝑛 + (1 + 𝑛+1 2 ) Δ𝐹𝑖 𝐷𝐴 Δ𝑡 𝑀𝑖 𝑛+1 = 𝑀𝑖 𝑛 + (1 + 𝑛+1 2 ) Δ𝑀𝑖 𝐷𝐵 Δ𝑡 The history variable labeled as “plastic strain” by LS-PrePost is actually volumetric strain in the case of *MAT_ELASTIC. Truss elements include a damping stress given by 𝜎 = 0.05𝜌𝑐𝐿/𝛥𝑡 where ρ is the mass density, 𝑐 is the material wave speed, 𝐿 is the element length, and 𝛥𝑡 is the computation time step. For the fluid option, the bulk modulus field, 𝐾, must be defined, and both the Young’s modulus and Poisson’s ratio fields are ignored. With the fluid option, fluid-like behavior is obtained where the bulk modulus, 𝐾, and pressure rate, 𝑝, are given by: 𝐾 = 3(1 − 2𝜈) 𝑝̇ = −𝐾𝜀̇𝑖𝑖 and the shear modulus is set to zero. A tensor viscosity is used which acts only the 𝑛+1, given in terms of the damping coefficient as: deviatoric stresses, 𝑆𝑖𝑗 𝑛+1 = VC × Δ𝐿 × 𝑎 × 𝜌𝜀̇𝑖𝑗 ′ 𝑆𝑖𝑗 where Δ𝐿 is a characteristic element length, 𝑎 is the fluid bulk sound speed, 𝜌 is the fluid density, and 𝜀̇𝑖𝑗 ′ is the deviatoric strain rate. *MAT_OPTIONTROPIC_ELASTIC This is Material Type 2. This material is valid for modeling the elastic-orthotropic behavior of solids, shells, and thick shells. An anisotropic option is available for solid elements. For orthotropic solids an isotropic frictional damping is available. In the case of solids, stresses are calculated not from incremental strains but rather from the deformation gradient. Also for solids, the elastic constants are formulated in terms of second Piola-Kirchhoff stress and Green’s strain, however, Cauchy stress is output. In the case of shells, the stress update is incremental and the elastic constants are formulated in terms of Cauchy stress and true strain. NOTE: This material does not support specification of a ma- terial angle, 𝛽𝑖, for each through-thickness integra- tion point of a shell. Available options include: ORTHO ANISO such that the keyword cards appear: *MAT_ORTHOTROPIC_ELASTIC or MAT_002 (4 cards follow) *MAT_ANISOTROPIC_ELASTIC or MAT_002_ANIS (5 cards follow) Orthotropic Card 1. Card 1 for ORTHO keyword option. Card 1 1 Variable MID 2 RO Type A8 F 3 EA F 4 EB F 5 EC F 6 7 8 PRBA PRCA PRCB F F F Orthotropic Card 2. Card 2 for ORTHO keyword option. Card 2 1 2 3 4 Variable GAB GBC GCA AOPT Type F F F F 5 G F 6 7 8 SIGF Anisotropic Card 1. Card 1 for ANISO keyword option. Card 1 1 Variable MID 2 RO 3 4 5 6 7 8 C11 C12 C22 C13 C23 C33 Type A8 F F F F F F F Anisotropic Card 2. Card 2 for ANISO keyword option. Card 2 1 2 3 4 5 6 7 8 Variable C14 C24 C34 C44 C15 C25 C35 C45 Type F F F F F F F F Anisotropic Card 3. Card 3 for ANISO keyword option. Card 3 1 2 3 4 5 6 7 8 Variable C55 C16 C26 C36 C46 C56 C66 AOPT Type F F F F F F F F Local Coordinate System Card 1. Required for all keyword options Card 4 Variable 1 XP Type F 2 YP F 3 ZP F 4 A1 F 5 A2 F 6 A3 F 7 8 MACF IHIS I Local Coordinate System Card 2. Required for all keyword options Card 5 Variable 1 V1 Type F 2 V2 F 3 V3 F 4 D1 F 5 D2 F 6 D3 F 7 8 BETA REF F F VARIABLE MID DESCRIPTION Material identification. A unique number or label not exceeding 8 characters must be specified. RO Mass density. Define for the ORTHO option only: EA EB EC PRBA PRCA PRCB GAB GBC GCA 𝐸𝑎, Young’s modulus in 𝑎-direction. 𝐸𝑏, Young’s modulus in 𝑏-direction. 𝐸𝑐, Young’s modulus in 𝑐-direction (nonzero value required but not used for shells). 𝜈𝑏𝑎, Poisson’s ratio in the 𝑏𝑎 direction. 𝜈𝑐𝑎, Poisson’s ratio in the 𝑐𝑎 direction. 𝜈𝑐𝑏, Poisson’s ratio in the 𝑐𝑏 direction. 𝐺𝑎𝑏, shear modulus in the 𝑎𝑏 direction. 𝐺𝑏𝑐, shear modulus in the 𝑏𝑐 direction. 𝐺𝑐𝑎, shear modulus in the 𝑐𝑎 direction. Due to symmetry define the upper triangular Cij’s for the ANISO option only: C11 C12 ⋮ C66 The 1, 1 term in the 6 × 6 anisotropic constitutive matrix. Note that 1 corresponds to the a material direction The 1, 2 term in the 6 × 6 anisotropic constitutive matrix. Note that 2 corresponds to the b material direction The 6, 6 term in the 6 × 6 anisotropic constitutive matrix. ⋮ Define AOPT for both options: AOPT Material axes option, see Figure M2-1. EQ.0.0: locally orthotropic with material axes determined by element nodes as shown in part (a) of Figure M2-1. The 𝐚-direction is from node 1 to node 2 of the element. The 𝐛-direction is orthogonal to the a-direction and is in the plane formed by nodes 1, 2, and 4. When this option is used in two-dimensional planar and axisym- metric analysis, it is critical that the nodes in the ele- ment definition be numbered counterclockwise for this option to work correctly. EQ.1.0: locally orthotropic with material axes determined by a point in space and the global location of the element center; this is the 𝐚-direction. This option is for solid elements only. EQ.2.0: globally orthotropic with material axes determined by vectors defined below, as with *DEFINE_COORDI- NATE_VECTOR. EQ.3.0: locally orthotropic material axes determined by rotating the material axes about the element normal by an angle, BETA, from a line in the plane of the element defined by the cross product of the vector 𝐯 with the element normal. The plane of a solid element is the midsurface between the inner surface and outer surface defined by the first four nodes and the last four nodes of the connectivity of the element, respectively. EQ.4.0: locally orthotropic in cylindrical coordinate system with the material axes determined by a vector 𝐯, and an originating point, 𝐏, which define the centerline ax- is. This option is for solid elements only. LT.0.0: the absolute value of AOPT is a coordinate system ID number (CID on *DEFINE_COORDINATE_NODES, *DEFINE_COORDINATE_SYSTEM or *DEFINE_CO- ORDINATE_VECTOR). Available in R3 version of 971 and later. G Shear modulus for frequency independent damping. Frequency independent damping is based of a spring and slider in series. The critical stress for the slider mechanism is SIGF defined below. For the best results, the value of G should be 250-1000 times greater than SIGF. This option applies only to solid elements. SIGF Limit stress for frequency independent, frictional, damping. XP, YP, ZP Define coordinates of point 𝐩 for AOPT = 1 and 4. A1, A2, A3 Define components of vector 𝐚 for AOPT = 2. MACF Material axes change flag for brick elements: EQ.1: No change, default, EQ.2: switch material axes 𝑎 and 𝑏, EQ.3: switch material axes 𝑎 and 𝑐, EQ.4: switch material axes 𝑏 and 𝑐. IHIS Flag for anisotropic stiffness terms initialization (for solid elements only). EQ.0: C11, C12, … from Cards 1, 2, and 3 are used. EQ.1: C11, C12, … are initialized by *INITIAL_STRESS_SOL- ID’s history data. V1, V2, V3 Define components of vector 𝐯 for AOPT = 3 and 4. D1, D2, D3 Define components of vector 𝐝 for AOPT = 2. BETA REF Material angle in degrees for AOPT = 3, may be overridden on the element card, see *ELEMENT_SHELL_BETA or *ELEMENT_- SOLID_ORTHO. Use reference geometry to initialize the stress tensor. The reference geometry is defined by the keyword: *INITIAL_- FOAM_REFERENCE_GEOMETRY . EQ.0.0: off, EQ.1.0: on. Remarks: The material law that relates stresses to strains is defined as: 𝐂 = 𝐓T𝐂𝐿𝐓 where 𝐓 is a transformation matrix, and 𝐂𝐿 is the constitutive matrix defined in terms of the material constants of the orthogonal material axes, {𝐚, 𝐛, 𝐜}. The inverse of 𝐂𝐿for the orthotropic case is defined as: −1 = 𝐂𝐿 𝐸𝑎 𝜐𝑎𝑏 𝐸𝑎 𝜐𝑎𝑐 𝐸𝑎 − − − − 𝜐𝑏𝑎 𝐸𝑏 𝐸𝑏 𝜐𝑏𝑐 𝐸𝑏 − − 𝜐𝑐𝑎 𝐸𝑐 𝜐𝑐𝑏 𝐸𝑐 𝐸𝑐 ⎡ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎣ 𝐺𝑎𝑏 𝐺𝑏𝑐 ⎤ ⎥ ⎥ ⎥ ⎥ ⎥ ⎥ ⎥ ⎥ ⎥ ⎥ ⎥ ⎥ ⎥ ⎥ ⎥ ⎥ 𝐺𝑐𝑎⎦ where, 𝜐𝑎𝑏 𝐸𝑎 = 𝜐𝑏𝑎 𝐸𝑏 , 𝜐𝑐𝑎 𝐸𝑐 = 𝜐𝑎𝑐 𝐸𝑎 , 𝜐𝑐𝑏 𝐸𝑐 = 𝜐𝑏𝑐 𝐸𝑏 . The frequency independent damping is obtained by having a spring and slider in series as shown in the following sketch: friction This option applies only to orthotropic solid elements and affects only the deviatoric stresses. The procedure for describing the principle material directions is now explained for solid and shell elements for this material model and other anisotropic materials. We will call the material coordinate system the {𝐚, 𝐛, 𝐜} coordinate system. The AOPT options illustrated in Figure M2-1 define the preliminary {𝐚, 𝐛, 𝐜} system for all elements of the parts that use the material, but this is not the final material direction. The {𝐚, 𝐛, 𝐜} system defined by the AOPT options may be offset by a final rotation about the 𝐜-axis. The offset angle we call BETA. For solid elements, the BETA angle is specified in one of two ways. When using AOPT = 3, the BETA parameter defines the offset angle for all elements that use the material. The BETA parameter has no meaning for the other AOPT options. Alternatively, a BETA angle can be defined for individual solid elements as described in remark 5 for *ELEMENT_SOLID_ORTHO. The beta angle by the ORTHO option is available for all values of AOPT, and it overrides the BETA angle on the *MAT card for AOPT = 3. The directions determined by the material AOPT options may be overridden for individual elements as described in remark 3 for *ELEMENT_SOLID_ORTHO. However, be aware that for materials with AOPT = 3, the final {𝐚, 𝐛, 𝐜} system will be the system defined on the element card rotated about 𝐜-axis by the BETA angle specified on the *MAT card. There are two fundamental differences between shell and solid element orthotropic materials. First, the 𝐜-direction is always normal to a shell element such that the 𝐚- direction and 𝐛-directions are within the plane of the element. Second, for some anisotropic materials, shell elements may have unique fiber directions within each layer through the thickness of the element so that a layered composite can be modeled with a single element. When AOPT = 0 is used in two-dimensional planar and axisymmetric analysis, it is critical that the nodes in the element definition be numbered counterclockwise for this option to work correctly. Because shell elements have their 𝐜-axes defined by the element normal, AOPT = 1 and AOPT = 4 are not available for shells. Also, AOPT = 2 requires only the vector 𝐚 be defined since 𝐝 is not used. The shell procedure projects the inputted 𝐚-direction onto each element surface. Similar to solid elements, the {𝐚, 𝐛, 𝐜} coordinate system determined by AOPT is then modified by a rotation about the 𝐜-axis which we will call 𝜙. For those materials that allow a unique rotation angle for each integration point through the element thickness, the rotation angle is calculated by 𝜙𝑖 = 𝛽 + 𝛽𝑖 where 𝛽 is a rotation for the element, and 𝛽𝑖 is the rotation for the i’th layer of the element. The 𝛽 angle can be input using the BETA parameter on the *MAT data, or will be overridden for individual elements if the BETA keyword option for *ELEMENT_- SHELL is used. The 𝛽𝑖 angles are input using the ICOMP = 1 option of *SECTION_- SHELL or with *PART_COMPOSITE. If 𝛽 or 𝛽𝑖 is omitted, they are assumed to be zero. All anisotropic shell materials have the BETA parameter on the *MAT card available for both AOPT = 0 and AOPT = 3, except for materials 91 and 92 which have it available (but called FANG instead of BETA) for AOPT = 0, 2, and 3. All anisotropic shell materials allow an angle for each integration point through the thickness, 𝛽𝑖, except for materials 2, 86, 91, 92, 117, 130, 170, 172, and 194. This discussion of material direction angles in shell elements also applies to thick shell elements which allow modeling of layered composites using *INTEGRATION_SHELL or *PART_COMPOSITE_TSHELL. Illustration of AOPT: Figure M2-1 AOPT = 0.0 AOPT = 1.0 (solid only) v14 c = a×b a = v12 b = v14 - a a⋅v14 a⋅a ⇒ a⋅b = 0 ez ey ex b = c x a d ∕∕ ez c = a x d a is set parallel to the line segment connecting p to the element center. d is set parallel to ez. input(p) → {a} → {c} → {b} AOPT = 2.0 (solid) AOPT = 2.0 (shell) c is orthogonal to the a,d plane c = a × d a,d are input. The computed axes do not depend on the element. b = c × a b is orthogonal to the c,a plane a = ainput - ⋅n ainput n⋅n c = n ainput b = c×a AOPT = 3.0 AOPT = 4.0 (solid only) c = n b = v - c c⋅v c⋅c a = b×n b is the projection of v (from input) onto the midplane/shell. Taken together, point p and vector v define the axis of symmetry. a = b×c b ∕∕ v c is parallel to the segment connecting the element center to the symmetry axis. (cid:13)(cid:51)(cid:36)(cid:53)(cid:55) (cid:66)(cid:77)(cid:84)(cid:109)(cid:105) (cid:98)(cid:118)(cid:75)(cid:35)(cid:81)(cid:72)(cid:103)(cid:47)(cid:50)(cid:98)(cid:43) (cid:84)(cid:66)(cid:47) (cid:75)(cid:66)(cid:47) (cid:99)(cid:51)(cid:106)(cid:99) (cid:66)(cid:47) (cid:56)(cid:82)(cid:97) (cid:106)(cid:64)(cid:67)(cid:99) (cid:85)(cid:29)(cid:97)(cid:106) (cid:85)(cid:82)(cid:67)(cid:78)(cid:106)(cid:51)(cid:97) (cid:106)(cid:82) (cid:76)(cid:29)(cid:106)(cid:51)(cid:97)(cid:67)(cid:29)(cid:73) (cid:13)(cid:40)(cid:47)(cid:40)(cid:48)(cid:40)(cid:49)(cid:55)(cid:66)(cid:54)(cid:50)(cid:47)(cid:44)(cid:39)(cid:66)(cid:94)(cid:50)(cid:51)(cid:55)(cid:44)(cid:50)(cid:49)(cid:96) (cid:66)(cid:77)(cid:84)(cid:109)(cid:105) (cid:98)(cid:118)(cid:75)(cid:35)(cid:81)(cid:72)(cid:103)(cid:47)(cid:50)(cid:98)(cid:43) (cid:84)(cid:66)(cid:47) (cid:35)(cid:50)(cid:105)(cid:28)(cid:103)(cid:28)(cid:83) (cid:86)(cid:28)(cid:83)(cid:87)(cid:46) (cid:28)(cid:108)(cid:46) (cid:28)(cid:107) (cid:47)(cid:83)(cid:46) (cid:47)(cid:108)(cid:46) (cid:47)(cid:107) (cid:85)(cid:82)(cid:67)(cid:78)(cid:106)(cid:51)(cid:97) (cid:106)(cid:82) (cid:85)(cid:29)(cid:97)(cid:106) (cid:1804)(cid:1397)(cid:46) (cid:48)(cid:51)(cid:56)(cid:29)(cid:110)(cid:73)(cid:106)(cid:99) (cid:106)(cid:82) (cid:122) (cid:531)(cid:1397)(cid:46) (cid:82)(cid:85)(cid:106)(cid:67)(cid:82)(cid:78)(cid:29)(cid:73) (cid:534)(cid:1397)(cid:46) (cid:82)(cid:85)(cid:106)(cid:67)(cid:82)(cid:78)(cid:29)(cid:73) (cid:105)(cid:64)(cid:51)(cid:78) (cid:73)(cid:51)(cid:106) (cid:531) (cid:30) (cid:531)(cid:1397) (cid:533) (cid:30) (cid:531)(cid:1397) (cid:3701) (cid:534)(cid:1397) (cid:532) (cid:30) (cid:533)(cid:1397) (cid:3701) (cid:531)(cid:1397)(cid:15) (cid:1804)(cid:1397) (cid:67)(cid:99) (cid:78)(cid:82)(cid:106) (cid:48)(cid:51)(cid:126)(cid:78)(cid:51)(cid:48)(cid:89) (cid:47)(cid:82)(cid:51)(cid:99) (cid:106)(cid:64)(cid:67)(cid:99) (cid:51)(cid:73)(cid:51)(cid:76)(cid:51)(cid:78)(cid:106) (cid:64)(cid:29)(cid:113)(cid:51) (cid:531)(cid:1397) (cid:29)(cid:78)(cid:48) (cid:534)(cid:1397)(cid:93) (cid:119)(cid:51)(cid:99) (cid:78)(cid:82) (cid:43)(cid:29)(cid:73)(cid:44)(cid:110)(cid:73)(cid:29)(cid:106)(cid:51) (cid:531)(cid:46) (cid:532)(cid:46) (cid:29)(cid:78)(cid:48) (cid:533) (cid:56)(cid:97)(cid:82)(cid:76) (cid:544)(cid:1429)(cid:46) (cid:531)(cid:1429)(cid:46) (cid:550)(cid:1429)(cid:46) (cid:29)(cid:78)(cid:48) (cid:534)(cid:1429) (cid:29)(cid:44)(cid:65) (cid:44)(cid:82)(cid:97)(cid:48)(cid:67)(cid:78)(cid:60) (cid:106)(cid:82) (cid:28)(cid:81)(cid:84)(cid:105) (cid:86)(cid:99)(cid:51)(cid:51) (cid:28)(cid:81)(cid:84)(cid:105) (cid:126)(cid:60)(cid:110)(cid:97)(cid:51)(cid:87)(cid:89) (cid:13)(cid:48)(cid:36)(cid:55) (cid:66)(cid:77)(cid:84)(cid:109)(cid:105) (cid:98)(cid:118)(cid:75)(cid:35)(cid:81)(cid:72)(cid:103)(cid:47)(cid:50)(cid:98)(cid:43) (cid:99)(cid:51)(cid:106) (cid:66)(cid:47) (cid:56)(cid:82)(cid:97) (cid:106)(cid:64)(cid:67)(cid:99) (cid:76)(cid:29)(cid:106)(cid:51)(cid:97)(cid:67)(cid:29)(cid:73) (cid:29)(cid:117)(cid:51)(cid:99) (cid:29)(cid:73)(cid:60)(cid:82)(cid:97)(cid:67)(cid:106)(cid:64)(cid:76) (cid:127)(cid:29)(cid:60) (cid:29)(cid:117)(cid:51)(cid:99) (cid:44)(cid:64)(cid:29)(cid:78)(cid:60)(cid:51) (cid:127)(cid:29)(cid:60) (cid:544)(cid:1429) (cid:531)(cid:1429) (cid:550)(cid:1429) (cid:534)(cid:1429) (cid:1804)(cid:1429)(cid:46) (cid:48)(cid:51)(cid:56)(cid:29)(cid:110)(cid:73)(cid:106)(cid:99) (cid:106)(cid:82) (cid:122) (cid:75)(cid:66)(cid:47) (cid:28)(cid:81)(cid:84)(cid:105) (cid:75)(cid:28)(cid:43)(cid:55) (cid:116)(cid:84)(cid:46) (cid:118)(cid:84)(cid:46) (cid:120)(cid:84) (cid:28)(cid:83)(cid:46) (cid:28)(cid:108)(cid:46) (cid:28)(cid:107) (cid:112)(cid:83)(cid:46) (cid:112)(cid:108)(cid:46) (cid:112)(cid:107) (cid:47)(cid:83)(cid:46) (cid:47)(cid:108)(cid:46) (cid:47)(cid:107) (cid:35)(cid:50)(cid:105)(cid:28) (cid:119)(cid:51)(cid:99) (cid:34)(cid:48)(cid:49)(cid:53) (cid:30) (cid:20)(cid:93) (cid:78)(cid:82) (cid:96)(cid:82)(cid:106)(cid:29)(cid:106)(cid:51) (cid:531) (cid:29)(cid:78)(cid:48) (cid:532) (cid:36)(cid:119) (cid:1804)(cid:1429) (cid:29)(cid:36)(cid:82)(cid:110)(cid:106) (cid:533)(cid:89) (cid:78)(cid:82) (cid:96)(cid:82)(cid:106)(cid:29)(cid:106)(cid:51) (cid:531) (cid:29)(cid:78)(cid:48) (cid:532) (cid:36)(cid:119) (cid:1804)(cid:1397) (cid:29)(cid:36)(cid:82)(cid:110)(cid:106) (cid:533)(cid:89) (cid:1804)(cid:1397) (cid:48)(cid:51)(cid:126)(cid:78)(cid:51)(cid:48)(cid:93) (cid:119)(cid:51)(cid:99) (cid:28)(cid:85)(cid:85)(cid:73)(cid:119) (cid:75)(cid:28)(cid:43)(cid:55)(cid:89) (cid:96)(cid:51)(cid:106)(cid:110)(cid:97)(cid:78) (cid:531)(cid:46) (cid:532)(cid:46) (cid:29)(cid:78)(cid:48) (cid:533)(cid:89) (cid:105)(cid:67)(cid:76)(cid:51) (cid:51)(cid:113)(cid:82)(cid:73)(cid:113)(cid:51) (cid:531)(cid:46) (cid:532)(cid:46) (cid:29)(cid:78)(cid:48) (cid:533) (cid:115)(cid:67)(cid:106)(cid:64) (cid:106)(cid:64)(cid:51) (cid:51)(cid:73)(cid:51)(cid:76)(cid:51)(cid:78)(cid:106)(cid:89) Figure M2-2. Flow chart showing how for each solid element LS-DYNA determines the vectors {𝒂, 𝒃, 𝒄} from the input. (cid:13)(cid:54)(cid:40)(cid:38)(cid:55)(cid:44)(cid:50)(cid:49)(cid:66)(cid:54)(cid:43)(cid:40)(cid:47)(cid:47) (cid:13)(cid:48)(cid:36)(cid:55) (cid:66)(cid:77)(cid:84)(cid:109)(cid:105) (cid:98)(cid:118)(cid:75)(cid:35)(cid:81)(cid:72)(cid:103)(cid:47)(cid:50)(cid:98)(cid:43) (cid:98)(cid:50)(cid:43)(cid:66)(cid:47) (cid:99)(cid:51)(cid:106)(cid:99) (cid:99)(cid:51)(cid:44)(cid:106)(cid:67)(cid:82)(cid:78) (cid:66)(cid:47) (cid:66)(cid:43)(cid:81)(cid:75)(cid:84) (cid:98)(cid:98)(cid:35)(cid:83)(cid:46) (cid:98)(cid:98)(cid:35)(cid:108)(cid:46) (cid:15)(cid:15)(cid:15) (cid:127)(cid:29)(cid:60)(cid:46) (cid:67)(cid:56) (cid:83) (cid:97)(cid:51)(cid:29)(cid:48) (cid:1804)(cid:1413) (cid:29)(cid:78)(cid:60)(cid:73)(cid:51)(cid:99)(cid:45) (cid:1804)(cid:1413)(cid:46) (cid:13)(cid:51)(cid:36)(cid:53)(cid:55) (cid:66)(cid:77)(cid:84)(cid:109)(cid:105) (cid:98)(cid:118)(cid:75)(cid:35)(cid:81)(cid:72)(cid:103)(cid:47)(cid:50)(cid:98)(cid:43) (cid:84)(cid:66)(cid:47) (cid:99)(cid:51)(cid:106) (cid:85)(cid:29)(cid:97)(cid:106) (cid:66)(cid:47) (cid:75)(cid:66)(cid:47) (cid:85)(cid:82)(cid:67)(cid:78)(cid:106)(cid:51)(cid:97) (cid:106)(cid:82) (cid:76)(cid:29)(cid:106)(cid:51)(cid:97)(cid:67)(cid:29)(cid:73) (cid:98)(cid:50)(cid:43)(cid:66)(cid:47) (cid:85)(cid:82)(cid:67)(cid:78)(cid:106)(cid:51)(cid:97) (cid:106)(cid:82) (cid:99)(cid:51)(cid:44)(cid:106)(cid:67)(cid:82)(cid:78) (cid:13)(cid:40)(cid:47)(cid:40)(cid:48)(cid:40)(cid:49)(cid:55)(cid:66)(cid:54)(cid:43)(cid:40)(cid:47)(cid:47)(cid:66)(cid:94)(cid:50)(cid:51)(cid:55)(cid:44)(cid:50)(cid:49)(cid:96) (cid:66)(cid:77)(cid:84)(cid:109)(cid:105) (cid:98)(cid:118)(cid:75)(cid:35)(cid:81)(cid:72)(cid:103)(cid:47)(cid:50)(cid:98)(cid:43) (cid:84)(cid:66)(cid:47) (cid:85)(cid:82)(cid:67)(cid:78)(cid:106)(cid:51)(cid:97) (cid:106)(cid:82) (cid:85)(cid:29)(cid:97)(cid:106) (cid:75)(cid:43)(cid:66)(cid:47) (cid:85)(cid:82)(cid:67)(cid:78)(cid:106)(cid:51)(cid:97) (cid:106)(cid:82) (cid:44)(cid:82)(cid:82)(cid:97)(cid:48)(cid:67)(cid:78)(cid:29)(cid:106)(cid:51) (cid:99)(cid:119)(cid:99)(cid:106)(cid:51)(cid:76) (cid:35)(cid:50)(cid:105)(cid:28) (cid:1804)(cid:1397)(cid:46) (cid:48)(cid:51)(cid:56)(cid:29)(cid:110)(cid:73)(cid:106)(cid:99) (cid:106)(cid:82) (cid:122) (cid:66)(cid:77)(cid:84)(cid:109)(cid:105) (cid:98)(cid:118)(cid:75)(cid:35)(cid:81)(cid:72)(cid:103)(cid:47)(cid:50)(cid:98)(cid:43) (cid:75)(cid:66)(cid:47) (cid:99)(cid:51)(cid:106)(cid:99) (cid:76)(cid:29)(cid:106)(cid:51)(cid:97)(cid:67)(cid:29)(cid:73) (cid:66)(cid:47) (cid:28)(cid:81)(cid:84)(cid:105) (cid:28)(cid:83)(cid:46) (cid:28)(cid:108)(cid:46) (cid:28)(cid:107) (cid:112)(cid:83)(cid:46) (cid:112)(cid:108)(cid:46) (cid:112)(cid:107) (cid:29)(cid:117)(cid:51)(cid:99) (cid:29)(cid:73)(cid:60)(cid:82)(cid:97)(cid:67)(cid:106)(cid:64)(cid:76) (cid:127)(cid:29)(cid:60) (cid:531)(cid:1429) (cid:550)(cid:1429) (cid:35)(cid:50)(cid:105)(cid:28) (cid:1804)(cid:1429)(cid:46) (cid:48)(cid:51)(cid:56)(cid:29)(cid:110)(cid:73)(cid:106)(cid:99) (cid:106)(cid:82) (cid:122) (cid:13)(cid:51)(cid:36)(cid:53)(cid:55)(cid:66)(cid:38)(cid:50)(cid:48)(cid:51)(cid:50)(cid:54)(cid:44)(cid:55)(cid:40) (cid:66)(cid:77)(cid:84)(cid:109)(cid:105) (cid:98)(cid:118)(cid:75)(cid:35)(cid:81)(cid:72)(cid:103)(cid:47)(cid:50)(cid:98)(cid:43) (cid:84)(cid:66)(cid:47) (cid:99)(cid:51)(cid:106)(cid:99) (cid:85)(cid:29)(cid:97)(cid:106) (cid:66)(cid:47) (cid:75)(cid:66)(cid:47)(cid:83)(cid:46) (cid:75)(cid:66)(cid:47)(cid:108)(cid:46) (cid:89)(cid:89)(cid:89) (cid:84)(cid:43)(cid:35)(cid:83)(cid:46) (cid:84)(cid:43)(cid:35)(cid:108)(cid:46) (cid:89)(cid:89)(cid:89) (cid:85)(cid:82)(cid:67)(cid:78)(cid:106)(cid:51)(cid:97) (cid:106)(cid:82) (cid:76)(cid:29)(cid:106)(cid:51)(cid:97)(cid:67)(cid:29)(cid:73) (cid:29)(cid:78)(cid:60)(cid:73)(cid:51)(cid:99)(cid:45) (cid:1804)(cid:1413) (cid:11)(cid:36)(cid:12) (cid:119)(cid:51)(cid:99) (cid:66)(cid:99) (cid:75)(cid:43)(cid:66)(cid:47) (cid:48)(cid:51)(cid:126)(cid:78)(cid:51)(cid:48)(cid:93) (cid:78)(cid:82) (cid:98)(cid:51)(cid:106) (cid:531)(cid:46) (cid:532)(cid:46) (cid:29)(cid:78)(cid:48) (cid:533) (cid:56)(cid:97)(cid:82)(cid:76) (cid:44)(cid:82)(cid:82)(cid:97)(cid:65) (cid:48)(cid:67)(cid:78)(cid:29)(cid:106)(cid:51) (cid:99)(cid:119)(cid:99)(cid:106)(cid:51)(cid:76) (cid:75)(cid:43)(cid:66)(cid:47)(cid:89) (cid:66)(cid:99) (cid:84)(cid:66)(cid:47) (cid:29) (cid:44)(cid:82)(cid:76)(cid:85)(cid:82)(cid:99)(cid:67)(cid:106)(cid:51)(cid:93) (cid:11)(cid:37)(cid:12) (cid:11)(cid:38)(cid:12) (cid:119)(cid:51)(cid:99) (cid:77) (cid:53) (cid:83) (cid:75) (cid:53) (cid:75)(cid:66)(cid:47)(cid:77) (cid:86)(cid:56)(cid:97)(cid:82)(cid:76) (cid:44)(cid:82)(cid:76)(cid:85)(cid:82)(cid:99)(cid:67)(cid:106)(cid:51)(cid:87) (cid:77) (cid:2957) (cid:77) (cid:90) (cid:83) (cid:78)(cid:82) (cid:75) (cid:53) (cid:75)(cid:66)(cid:47) (cid:86)(cid:56)(cid:97)(cid:82)(cid:76) (cid:84)(cid:28)(cid:96)(cid:105)(cid:87) (cid:78)(cid:82) (cid:43)(cid:29)(cid:73)(cid:44)(cid:110)(cid:73)(cid:29)(cid:106)(cid:51) (cid:531)(cid:46) (cid:532)(cid:46) (cid:29)(cid:78)(cid:48) (cid:533) (cid:56)(cid:97)(cid:82)(cid:76) (cid:531)(cid:1429) (cid:29)(cid:78)(cid:48) (cid:550)(cid:1429) (cid:29)(cid:44)(cid:44)(cid:82)(cid:97)(cid:48)(cid:67)(cid:78)(cid:60) (cid:106)(cid:82) (cid:28)(cid:81)(cid:84)(cid:105) (cid:56)(cid:82)(cid:97) (cid:76)(cid:29)(cid:106)(cid:51)(cid:97)(cid:67)(cid:29)(cid:73) (cid:75) (cid:86)(cid:99)(cid:51)(cid:51) (cid:28)(cid:81)(cid:84)(cid:105) (cid:126)(cid:60)(cid:110)(cid:97)(cid:51)(cid:87)(cid:89) (cid:66)(cid:99) (cid:76)(cid:29)(cid:106)(cid:51)(cid:97)(cid:67)(cid:29)(cid:73) (cid:75) (cid:29)(cid:78)(cid:67)(cid:99)(cid:82)(cid:106)(cid:97)(cid:82)(cid:85)(cid:67)(cid:44)(cid:93) (cid:119)(cid:51)(cid:99) (cid:28)(cid:81)(cid:84)(cid:105) (cid:67)(cid:99) (cid:51)(cid:67)(cid:106)(cid:64)(cid:51)(cid:97) (cid:122) (cid:82)(cid:97) (cid:107)(cid:93) (cid:119)(cid:51)(cid:99) (cid:1804)(cid:1397) (cid:48)(cid:51)(cid:126)(cid:78)(cid:51)(cid:48)(cid:93) (cid:119)(cid:51)(cid:99) (cid:1804) (cid:53) (cid:1804)(cid:1397) (cid:1804) (cid:53) (cid:1804)(cid:1429) (cid:78)(cid:82) (cid:96)(cid:82)(cid:106)(cid:29)(cid:106)(cid:51) (cid:531) (cid:29)(cid:78)(cid:48) (cid:532) (cid:36)(cid:119) (cid:1804) (cid:29)(cid:36)(cid:82)(cid:110)(cid:106) (cid:533)(cid:89) (cid:78)(cid:82) (cid:72)(cid:51)(cid:106) (cid:1804)(cid:1429) (cid:30) (cid:17) (cid:11)(cid:39)(cid:12) (cid:98)(cid:51)(cid:106) (cid:29)(cid:73)(cid:73) (cid:92)(cid:1804)(cid:94)(cid:1413) (cid:30) (cid:17) (cid:92)(cid:1804)(cid:1413)(cid:94) (cid:30) (cid:92)(cid:458)(cid:445)(cid:444)(cid:451)(cid:94) (cid:92)(cid:1804)(cid:1413)(cid:94) (cid:30) (cid:92)(cid:461)(cid:461)(cid:444)(cid:451)(cid:94) (cid:119)(cid:51)(cid:99) (cid:119)(cid:51)(cid:99) (cid:66)(cid:99) (cid:84)(cid:66)(cid:47) (cid:29) (cid:44)(cid:82)(cid:76)(cid:85)(cid:82)(cid:99)(cid:67)(cid:106)(cid:51)(cid:93) (cid:78)(cid:82) (cid:66)(cid:43)(cid:81)(cid:75)(cid:84) (cid:53) (cid:83)(cid:93) (cid:78)(cid:82) (cid:105)(cid:67)(cid:76)(cid:51) (cid:51)(cid:113)(cid:82)(cid:73)(cid:113)(cid:51) (cid:531)(cid:46) (cid:532)(cid:46) (cid:533)(cid:46) (cid:29)(cid:78)(cid:48) (cid:92)(cid:1804)(cid:1413)(cid:94)(cid:89) (cid:96)(cid:51)(cid:106)(cid:110)(cid:97)(cid:78) (cid:531)(cid:46) (cid:532)(cid:46) (cid:533)(cid:46) (cid:29)(cid:78)(cid:48) (cid:92)(cid:1804)(cid:1413)(cid:94)(cid:89) Figure M2-3. Flowchart for shells: (a) check for coordinate system ID; (b) process AOPT; (c) deterimine 𝛽; and (d) for each layer determine 𝛽𝑖. *MAT_003 This is Material Type 3. This model is suited to model isotropic and kinematic hardening plasticity with the option of including rate effects. It is a very cost effective model and is available for beam (Hughes-Liu and Truss), shell, and solid elements. Card 1 1 Variable MID 2 RO Type A8 F 3 E F 4 PR F 5 6 7 8 SIGY ETAN BETA F F F Default none none none none none 0.0 0.0 5 6 7 8 Card 2 1 2 Variable SRC SRP Type F F 3 FS F 4 VP F Default 0.0 0.0 1.E+20 0.0 VARIABLE DESCRIPTION MID RO E PR SIGY ETAN BETA SRC Material identification. A unique number or label not exceeding 8 characters must be specified. Mass density. Young’s modulus. Poisson’s ratio. Yield stress. Tangent modulus, see Figure M3-1 Hardening parameter, 0 < 𝛽′ < 1. See comments below. Strain rate parameter, C, for Cowper Symonds strain rate model, see below. If zero, rate effects are not considered.. Et Yield Stress ⎛ ⎜ ⎝ ⎛ ⎜ ⎝ l0 ln β=0, kinematic hardening β=1, isotropic hardening Figure M3-1. Elastic-plastic behavior with kinematic and isotropic hardening where 𝑙0 and 𝑙 are undeformed and deformed lengths of uniaxial tension specimen. 𝐸𝑡 is the slope of the bilinear stress strain curve. VARIABLE DESCRIPTION Strain rate parameter, P, for Cowper Symonds strain rate model, see below. If zero, rate effects are not considered. Effective plastic strain for eroding elements. Formulation for rate effects: EQ.0.0: Scale yield stress (default), EQ.1.0: Viscoplastic formulation (recommended) SRP FS VP Remarks: Strain rate is accounted for using the Cowper and Symonds model which scales the yield stress with the factor 1 + ( 𝜀̇ 𝑝⁄ ) where 𝜀̇ is the strain rate. A fully viscoplastic formulation is optional which incorporates the Cowper and Symonds formulation within the yield surface. To ignore strain rate effects set both SRC and SRP to zero. Kinematic, isotropic, or a combination of kinematic and isotropic hardening may be specified by varying 𝛽′ between 0 and 1. For 𝛽′ equal to 0 and 1, respectively, kinematic and isotropic hardening are obtained as shown in Figure M3-1. For isotropic hardening, 𝛽′= 1, Material Model 12, *MAT_ISOTROPIC_ELASTIC_PLASTIC, requires less storage and is more efficient. Whenever possible, Material 12 is recommended for solid elements, but for shell elements it is less accurate and thus Material 12 is not recommended in this case. *MAT_ELASTIC_PLASTIC_THERMAL This is Material Type 4. Temperature dependent material coefficients can be defined. A maximum of eight temperatures with the corresponding data can be defined. A minimum of two points is needed. When this material type is used it is necessary to define nodal temperatures by activating a coupled analysis or by using another option to define the temperatures such as *LOAD_THERMAL_LOAD_CURVE, or *LOAD_- THERMAL_VARIABLE. Card 1 1 Variable MID 2 RO Type A8 F Card 2 Variable 1 T1 Type F Card 3 Variable 1 E1 Type F Card 4 1 2 T2 F 2 E2 F 2 3 4 5 6 7 8 3 T3 F 3 E3 F 3 4 T4 F 4 E4 F 4 5 T5 F 5 E5 F 5 6 T6 F 6 E6 F 6 7 T7 F 7 E7 F 7 8 T8 F 8 E8 F 8 Variable PR1 PR2 PR3 PR4 PR5 PR6 PR7 PR8 Type F F F F F F F No defaults are assumed. Card 5 1 2 3 4 5 6 7 8 Variable ALPHA1 ALPHA2 ALPHA3 ALPHA4 ALPHA5 ALPHA6 ALPHA7 ALPHA8 Type F Card 6 1 F 2 F 3 F 4 F 5 F 6 F 7 F 8 Variable SIGY1 SIGY2 SIGY3 SIGY4 SIGY5 SIGY6 SIGY7 SIGY8 Type F Card 7 1 F 2 F 3 F 4 F 5 F 6 F 7 F 8 Variable ETAN1 ETAN2 ETAN3 ETAN4 ETAN5 ETAN6 ETAN7 ETAN8 Type F F F F F F F F VARIABLE DESCRIPTION MID RO TI EI PRI Material identification. A unique number or label not exceeding 8 characters must be specified. Mass density. Temperatures. The minimum is 2, the maximum is 8. Corresponding Young’s moduli at temperature TI. Corresponding Poisson’s ratios. ALPHAI Corresponding coefficients of thermal expansion. SIGYI Corresponding yield stresses. ETANI Corresponding plastic hardening moduli. *MAT_ELASTIC_PLASTIC_THERMAL The stress update for this material follows the standard approach to hypo- elastoplasticity, using Jaumann rate for objectivity. The rate of Cauchy stress 𝝈 can in principal be expressed as 𝝈̇ = 𝑪(𝜺̇ − 𝜺̇𝑇 − 𝜺̇𝑝) + 𝑪̇𝑪−1𝝈 where 𝑪 is the temperature dependent isotropic elasticity tensor, 𝜺̇ is the rate-of- deformation, 𝜺̇𝑇 is the thermal strain rate and 𝜺̇𝑝 is the plastic strain rate. The coefficient of thermal expansion is defined as the instantaneous value. Thus, the thermal strain rate becomes 𝜺̇𝑇 = 𝛼𝑇̇𝑰 where 𝛼 is the temperature dependent thermal expansion coefficient, 𝑇̇ is the rate of temperature and 𝑰 is the identity tensor. Associated von Mises plasticity is adopted, resulting in 𝜺̇𝑝 = 𝜀̇𝑝 3𝒔 2𝜎̅̅̅̅̅ where 𝜀̇𝑝 is the effective plastic strain rate, 𝒔 is the deviatoric stress tensor and 𝜎̅̅̅̅̅ is the von Mises effective stress. The last term accounts for stress changes due to change in stiffness with respect to temperature, using the total elastic strain defined as 𝜺𝑒 = 𝑪−1𝝈. A way to intuitively understand this contribution, for small displacement elasticity if neglecting everything but the temperature dependent elasticity parameters, we have 𝝈̇ = 𝑑𝑡 (𝑪𝜺) as a special case, showing that the stress may change without any change in strain. At least two temperatures and their corresponding material properties must be defined. The analysis will be terminated if a material temperature falls outside the range defined in the input. If a thermo-elastic material is considered, do not define SIGY and ETAN. *MAT_005 This is Material Type 5. It is a relatively simple material model for representing soil, concrete, or crushable foam. A table can be defined if thermal effects are considered in the pressure versus volumetric strain behavior. Card 1 1 Variable MID Type A8 Card 2 1 2 RO F 2 3 G F 3 4 KUN F 4 5 A0 F 5 6 A1 F 6 7 A2 F 7 8 PC F 8 Variable VCR REF LCID Type F Card 3 1 F 2 F 3 4 5 6 7 8 Variable EPS1 EPS2 EPS3 EPS4 EPS5 EPS6 EPS7 EPS8 Type F Card 4 1 F 2 Variable EPS9 EPS10 Type F F Card 5 Variable 1 P1 Type F 2 P2 F F 3 3 P3 F F 4 4 P4 F F 5 5 P5 F F 6 6 P6 F F 7 7 P7 F F 8 8 P8 4 5 6 7 8 *MAT_005 Card 6 Variable 1 P9 2 P10 Type F F VARIABLE DESCRIPTION MID RO G Material identification. A unique number or label not exceeding 8 characters must be specified. Mass density. Shear modulus. KUN Bulk modulus for unloading used for VCR = 0.0. A0 A1 A2 PC Yield function constant for plastic yield function below. Yield function constant for plastic yield function below. Yield function constant for plastic yield function below. Pressure cutoff for tensile fracture (< 0). VCR Volumetric crushing option: EQ.0.0: on, EQ.1.0: loading and unloading paths are the same. REF Use reference geometry to initialize the pressure. The reference geometry is defined by the keyword:*INITIAL_FOAM_REFER- ENCE_GEOMETRY. the deviatoric stress state. This option does not initialize EQ.0.0: off, EQ.1.0: on. VARIABLE LCID EPS1, … DESCRIPTION Load curve ID for compressive pressure (ordinate) as a function of volumetric strain (abscissa). If LCID is defined, then the curve is used instead of the input for EPS1…, and P1…. It makes no difference whether the values of volumetric strain in the curve are input as positive or negative since internally, a negative sign is applied to the absolute value of each abscissa entry. The response is extended to being temperature dependent if LCID refers to a table. Volumetric strain values in pressure vs. volumetric strain curve . A maximum of 10 values including 0.0 are allowed and a minimum of 2 values are necessary. If EPS1 is not 0.0 then a point (0.0, 0.0) will be automatically generated and a maximum of nine values may be input. P1, P2, …, PN Pressures corresponding to volumetric strain values given on Cards 3 and 4. Loading and unloading (along the grey arows) follows the input curve when the volumetric crushing option is off (VCR = 1.0) tension Pressure Cutoff Value compression Volumetric Strain, ln ⎛ ⎜ ⎝ ⎛ ⎜ ⎝ V0 The bulk unloading modulus is used if the volumetric crushing option is on (VCR = 0). In thiscase the aterial's response follows the black arrows. Figure M5-1. Pressure versus volumetric strain curve for soil and crushable foam model. The volumetric strain is given by the natural logarithm of the relative volume, 𝑉. Remarks: Pressure is positive in compression. Volumetric strain is given by the natural log of the relative volume and is negative in compression. Relative volume is a ratio of the current volume to the initial volume at the start of the calculation. The tabulated data should be given in order of increasing compression. If the pressure drops below the cutoff value specified, it is reset to that value. For a detailed description we refer to Kreig [1972]. The deviatoric perfectly plastic yield function, 𝜙, is described in terms of the second invariant 𝐽2, 𝐽2 = 𝑠𝑖𝑗𝑠𝑖𝑗, pressure, 𝑝, and constants 𝑎0, 𝑎1, and 𝑎2 as: 𝜙 = 𝐽2 − [𝑎0 + 𝑎1𝑝 + 𝑎2𝑝2]. On the yield surface 𝐽2 = 1 3 𝜎𝑦 2 where 𝜎𝑦 is the uniaxial yield stress, i.e., there is no strain hardening on this surface. 𝜎𝑦 = [3(𝑎0 + 𝑎1𝑝 + 𝑎2𝑝2)] 2⁄ To eliminate the pressure dependence of the yield strength, set: 𝑎1 = 𝑎2 = 0 and 𝑎0 = 2. 𝜎𝑦 This approach is useful when a von Mises type elastic-plastic model is desired for use with the tabulated volumetric data. The history variable labeled as “plastic strain” by LS-PrePost is actually plastic volumetric strain. Note that when VCR = 1.0, plastic volumetric strain is zero. *MAT_VISCOELASTIC This is Material Type 6. This model allows the modeling of viscoelastic behavior for beams (Hughes-Liu), shells, and solids. Also see *MAT_GENERAL_VISCOELASTIC for a more general formulation. Card 1 1 Variable MID 2 RO 3 BULK Type A8 F F 6 7 8 BETA F 4 G0 F 5 GI F DESCRIPTION VARIABLE MID Material identification. A unique number or label not exceeding 8 characters must be specified. RO Mass density BULK Elastic bulk modulus. LT.0.0: |BULK| is load curve of bulk modulus as a function of temperature. G0 Short-time shear modulus, see equations below. LT.0.0: |G0| is load curve of short-time shear modulus as a function of temperature. GI Long-time (infinite) shear modulus, G∞. LT.0.0: |GI| is load curve of long-time shear modulus as a function of temperature. BETA Decay constant. LT.0.0: |BETA| is load curve of decay constant as a function of temperature. Remarks: The shear relaxation behavior is described by [Hermann and Peterson, 1968]: A Jaumann rate formulation is used 𝐺(𝑡) = 𝐺∞ + (𝐺0 − 𝐺∞)exp (−𝛽𝑡) ∇ ′ = 2 ∫ 𝐺(𝑡 − 𝜏)𝐷′𝑖𝑗(𝜏)𝑑𝜏 ij ∇ 𝑖𝑗, and the strain rate, D𝑖𝑗. where the prime denotes the deviatoric part of the stress rate, 𝜎 *MAT_BLATZ-KO_RUBBER This is Material Type 7. This one parameter material allows the modeling of nearly incompressible continuum rubber. The Poisson’s ratio is fixed to 0.463. Card 1 1 Variable MID 2 RO Type A8 F 3 G F 4 REF F 5 6 7 8 VARIABLE DESCRIPTION MID RO G REF Material identification. A unique number or label not exceeding 8 characters must be specified. Mass density. Shear modulus. Use reference geometry to initialize the stress tensor. The reference geometry is defined by the keyword:*INITIAL_FOAM_- REFERENCE_GEOMETRY . EQ.0.0: off, EQ.1.0: on. Remarks: The strain energy density potential for the Blatz-Ko rubber is 𝑊(𝐂) = [𝐼1 − 3 + −𝛽 − 1)] (𝐼3 where 𝐺 is the shear modulus, 𝐼1 and 𝐼3 are the first and third invariants of the right Cauchy-Green tensor 𝐂 = 𝐅T𝐅 and 1 − 2𝑣 The second Piola-Kirchhoff stress is computed as 𝛽 = . 𝐒 = 2 𝜕𝑊 𝜕𝐂 = 𝐺[𝐈 − 𝐼3 −𝛽𝐂−1] from which the Cauchy stress is obtained by a push-forward from the reference to current configuration divided by the relative volume 𝐽 = det(𝑭), 𝛔 = 𝐅𝐒𝐅T = [𝐁 − 𝐼3 −𝛽𝐈]. Here we used 𝐁 = 𝐅𝐅T to denote the left Cauchy-Green tensor, and the Poisson ratio 𝑣 above is set internally to 𝑣 = 0.463, also see Blatz and Ko [1962]. *MAT_HIGH_EXPLOSIVE_BURN This is Material Type 8. It allows the modeling of the detonation of a high explosive. In addition an equation of state must be defined. See Wilkins [1969] and Giroux [1973]. Card 1 1 Variable MID 2 RO Type A8 F 3 D F 4 5 PCJ BETA F F 6 K F 7 G F 8 SIGY F VARIABLE DESCRIPTION MID RO D PCJ Material identification. A unique number or label not exceeding 8 characters must be specified. Mass density. Detonation velocity. Chapman-Jouget pressure. BETA Beta burn flag, BETA : EQ.0.0: beta and programmed burn, EQ.1.0: beta burn only, EQ.2.0: programmed burn only. K G Bulk modulus (BETA = 2.0 only). Shear modulus (BETA = 2.0 only). SIGY 𝜎y, yield stress (BETA = 2.0 only). Remarks: Burn fractions, 𝐹, which multiply the equations of states for high explosives, control the release of chemical energy for simulating detonations. At any time, the pressure in a high explosive element is given by: where 𝑝eos, is the pressure from the equation of state (either types 2, 3, or 14), V is the relative volume, and E is the internal energy density per unit initial volume. 𝑝 = 𝐹𝑝eos(𝑉, 𝐸) In the initialization phase, a lighting time tl is computed for each element by dividing the distance from the detonation point to the center of the element by the detonation velocity D. If multiple detonation points are defined, the closest detonation point determines tl. The burn fraction 𝐹 is taken as the maximum Where 𝐹 = max(𝐹1, 𝐹2) 𝐹1 = ⎧2 (𝑡 − 𝑡𝑙)𝐷𝐴𝑒max { 3𝑣𝑒 ⎨ { 0 ⎩ if 𝑡 > 𝑡𝑙 if 𝑡 ≤ 𝑡𝑙 𝐹2 = 𝛽 = 1 − 𝑉 1 − 𝑉𝐶𝐽 where 𝑉𝐶𝐽 is the Chapman-Jouguet relative volume and t is current time. If 𝐹 exceeds 1, it is reset to 1. This calculation of the burn fraction usually requires several time steps for 𝐹 to reach unity, thereby spreading the burn front over several elements. After reaching unity, 𝐹 is held constant. This burn fraction calculation is based on work by Wilkins [1964] and is also discussed by Giroux [1973]. If the beta burn option is used, BETA = 1.0, any volumetric compression will cause detonation and and 𝐹1 is not computed. 𝐹 = 𝐹2 If programmed burn is used, BETA = 2.0, the undetonated high explosive material will behave as an elastic perfectly plastic material if the bulk modulus, shear modulus, and yield stress are defined. Therefore, with this option the explosive material can compress without causing detonation. The location and time of detonation is controlled by *INITIAL_DETONATION. As an option, the high explosive material can behave as an elastic perfectly-plastic solid prior to detonation. In this case we update the stress tensor, to an elastic trial stress, ∗ 𝑠𝑖𝑗 𝑛+1, ∗ 𝑠𝑖𝑗 𝑛+1 = 𝑠𝑖𝑗 𝑛 + 𝑠𝑖𝑝𝛺𝑝𝑗 + 𝑠𝑗𝑝𝛺𝑝𝑖 + 2𝐺𝜀′̇ 𝑖𝑗𝑑𝑡 where 𝐺 is the shear modulus, and 𝜀′̇ condition is given by: 𝑖𝑗 is the deviatoric strain rate. The von Mises yield 𝜙 = 𝐽2 − 𝜎𝑦 where the second stress invariant, 𝐽2, is defined in terms of the deviatoric stress components as and the yield stress is 𝜎𝑦. If yielding has occurred, i.e., 𝜑 > 0, the deviatoric trial stress is scaled to obtain the final deviatoric stress at time n+1: 𝑠𝑖𝑗𝑠𝑖𝑗 𝐽2 = If 𝜑 ≤ 0, then 𝑛+1 = 𝑠𝑖𝑗 𝜎𝑦 √3𝐽2 ∗ 𝑠𝑖𝑗 𝑛+1 𝑛+1 =∗ 𝑠𝑖𝑗 𝑠𝑖𝑗 𝑛+1 Before detonation pressure is given by the expression 𝑝𝑛+1 = Κ ( 𝑉𝑛+1 − 1) where K is the bulk modulus. Once the explosive material detonates: and the material behaves like a gas. 𝑛+1 = 0 𝑠𝑖𝑗 This is Material Type 9. *MAT_009 In the case of solids and thick shells, this material allows equations of state to be considered without computing deviatoric stresses. Optionally, a viscosity can be defined. Also, erosion in tension and compression is possible. Beams and shells that use this material type are completely bypassed in the element processing; however, the mass of the null beam or shell elements is computed and added to the nodal points which define the connectivity. The mass of null beams is ignored if the value of the density is less than 1.e-11. The Young’s modulus and Poisson’s ratio are used only for setting the contact stiffness, and it is recommended that reasonable values be input. The variables PC, MU, TEROD, and EDROD do not apply to beams and shells. Historically, null beams and/or null shells have been used as an aid in modeling of contact but this practice is now seldom needed. Card 1 1 Variable MID 2 RO Type A8 F 3 PC F 4 5 6 7 MU TEROD CEROD YM F F F F 8 PR F Defaults none none 0.0 0.0 0.0 0.0 0.0 0.0 VARIABLE DESCRIPTION MID RO PC MU TEROD CEROD Material identification. A unique number or label not exceeding 8 characters must be specified. Mass density Pressure cutoff (≤ 0.0). See Remark 4. Dynamic viscosity μ (optional). See Remark 1. Relative volume. 𝑉 𝑉0 greater than unity. If zero, erosion in tension is inactive. , for erosion in tension. Typically, use values Relative volume, 𝑉 𝑉0 values less than unity. If zero, erosion in compression is inactive. , for erosion in compression. Typically, use YM Young’s modulus (used for null beams and shells only) *MAT_NULL DESCRIPTION PR Poisson’s ratio (used for null beams and shells only) Remarks: These remarks apply to solids and thick shells only. 1. When used with solids or thick shells, this material must be used with an equation-of-state. Pressure cutoff is negative in tension. A (deviatoric) viscous stress of the form 𝜎′𝑖𝑗 = 2𝜇𝜀′̇ 𝑚2 𝑠] [ 𝑚2] ~ [ is computed for nonzero 𝜇 where 𝜀′̇ 𝑖𝑗 is the deviatoric strain rate. 𝜇 is the dy- namic viscosity. For example, in SI unit system, 𝜇 may have a unit of [Pa*s]. 𝑖𝑗 ] [ 2. Null material has no shear stiffness (except from viscosity) and hourglass control must be used with great care. In some applications, the default hour- glass coefficient may lead to significant energy losses. In general for fluid, the hourglass coefficient QM should be small (in the range 1.0E-6 to 1.0E-4) and the hourglass type IHQ should be set to 1 (default). 3. The Null material has no yield strength and behaves in a fluid-like manner. 4. The cut-off pressure, PC, must be defined to allow for a material to “numerical- ly” cavitate. In other words, when a material undergoes dilatation above cer- tain magnitude, it should no longer be able to resist this dilatation. Since dilatation stress or pressure is negative, setting PC limit to a very small negative number would allow for the material to cavitate once the pressure in the mate- rial goes below this negative value. *MAT_ELASTIC_PLASTIC_HYDRO_{OPTION} This is Material Type 10. This material allows the modeling of an elastic-plastic hydrodynamic material and requires an equation-of-state (*EOS). Available options include: <BLANK> SPALL STOCHASTIC The keyword card can appear in two ways: *MAT_ELASTIC_PLASTIC_HYDRO or MAT_010 *MAT_ELASTIC_PLASTIC_HYDRO_SPALL or MAT_010_SPALL Card 1 1 Variable MID 2 RO Type A8 F 3 G F 4 SIG0 F 5 EH F Default none none none 0.0 0.0 6 PC F -∞ 7 FS F 8 CHARL F 0.0 0.0 Spall Card. Additional card for SPALL keyword option. Optional Variable 1 A1 Type F Card 2 1 2 A2 F 2 3 4 5 6 7 8 SPALL F 3 4 5 6 7 8 Variable EPS1 EPS2 EPS3 EPS4 EPS5 EPS6 EPS7 EPS8 Type F F F F F F F Card 3 1 2 3 4 5 6 7 8 Variable EPS9 EPS10 EPS11 EPS12 EPS13 EPS14 EPS15 EPS16 Type F Card 4 1 F 2 F 3 F 4 F 5 F 6 F 7 F 8 Variable ES1 ES2 ES3 ES4 ES5 ES6 ES7 ES8 Type F Card 5 1 F 2 F 3 F 4 F 5 F 6 F 7 F 8 Variable ES9 ES10 ES11 ES12 ES13 ES14 ES15 ES16 Type F F F F F F F F VARIABLE DESCRIPTION MID RO G Material identification. A unique number or label not exceeding 8 characters must be specified. Mass density. Shear modulus. SIG0 Yield stress, see comment below. EH PC FS Plastic hardening modulus, see definition below. Pressure cutoff (≤ 0.0). If zero, a cutoff of -∞ is assumed. Effective plastic strain at which erosion occurs. Piecewise linear curve defining the yield stress versus effective plastic strain. As illustrated, the yield stress at zero plastic strain should be nonzero. ep Figure M10-1. Effective stress versus effective plastic strain curve. See EPS and ES input. VARIABLE CHARL DESCRIPTION Characteristic element thickness for deletion. This applies to 2D solid elements that lie on a boundary of a part. If the boundary element thins down due to stretching or compression, and if it thins to a value less than CHARL, the element will be deleted. The primary application of this option is to predict the break-up of axisymmetric shaped charge jets. A1 A2 Linear pressure hardening coefficient. Quadratic pressure hardening coefficient. SPALL Spall type: EQ.0.0: default set to “1.0”, EQ.1.0: tensile pressure is limited by PC, i.e., p is always ≥ PC, EQ.2.0: if 𝜎max ≥ −PC element spalls and tension, 𝑝 < 0, is never allowed, EQ.3.0: 𝑝 < PC element spalls and tension, 𝑝 < 0, is never allowed. EPS Effective plastic strain (True). Define up to 16 values. Care must be taken that the full range of strains expected in the analysis is covered. Linear extrapolation is used if the strain values exceed the maximum input value. ES Effective stress. Define up to 16 values. *MAT_ELASTIC_PLASTIC_HYDRO If ES and EPS are undefined, the yield stress and plastic hardening modulus are taken from SIG0 and EH. In this case, the bilinear stress-strain curve shown in M10-1 is obtained with hardening parameter, 𝛽 = 1. The yield strength is calculated as 𝜎𝑦 = 𝜎0 + 𝐸ℎ𝜀̅𝑝 + (𝑎1 + 𝑝𝑎2)max[𝑝, 0] The quantity 𝐸ℎ is the plastic hardening modulus defined in terms of Young’s modulus, 𝐸, and the tangent modulus, 𝐸𝑡, as follows and 𝑝 is the pressure taken as positive in compression. 𝐸ℎ = 𝐸𝑡𝐸 𝐸 − 𝐸𝑡 . If ES and EPS are specified, a curve like that shown in M10-1 may be defined. Effective stress is defined in terms of the deviatoric stress tensor, 𝑠𝑖𝑗, as: 𝜎̅̅̅̅̅ = ( 2⁄ 𝑠𝑖𝑗𝑠𝑖𝑗) and effective plastic strain by: 𝜀̅𝑝 = ∫ ( 2⁄ 𝑝 ) 𝑝 𝐷𝑖𝑗 𝐷𝑖𝑗 𝑑𝑡, 𝑝 is the plastic component of the rate of deformation tensor. where t denotes time and 𝐷𝑖𝑗 In this case the plastic hardening modulus on Card 1 is ignored and the yield stress is given as where the value for 𝑓 (𝜀̅𝑝) is found by interpolation from the data curve. 𝜎𝑦 = 𝑓 (𝜀̅𝑝), A choice of three spall models is offered to represent material splitting, cracking, and failure under tensile loads. The pressure limit model, SPALL = 1, limits the hydrostatic tension to the specified value, 𝑝cut. If pressures more tensile than this limit are calculated, the pressure is reset to pcut. This option is not strictly a spall model, since the deviatoric stresses are unaffected by the pressure reaching the tensile cutoff, and the pressure cutoff value, pcut, remains unchanged throughout the analysis. The maximum principal stress spall model, SPALL = 2, detects spall if the maximum principal stress, 𝜎max, exceeds the limiting value -𝑝cut. Note that the negative sign is required because 𝑝cut is measured positive in compression, while 𝜎max is positive in tension. Once spall is detected with this model, the deviatoric stresses are reset to zero, and no hydrostatic tension (𝑝 < 0) is permitted. If tensile pressures are calculated, they are reset to 0 in the spalled material. Thus, the spalled material behaves as a rubble or incohesive material. The hydrostatic tension spall model, SPALL = 3, detects spall if the pressure becomes more tensile than the specified limit, 𝑝cut. Once spall is detected the deviatoric stresses are reset to zero, and nonzero values of pressure are required to be compressive (positive). If hydrostatic tension (𝑝 < 0) is subsequently calculated, the pressure is reset to 0 for that element. This model is applicable to a wide range of materials, including those with pressure- dependent yield behavior. The use of 16 points in the yield stress versus effective plastic strain curve allows complex post-yield hardening behavior to be accurately represented. In addition, the incorporation of an equation of state permits accurate modeling of a variety of different materials. The spall model options permit incorporation of material failure, fracture, and disintegration effects under tensile loads. The STOCHASTIC option allows spatially varying yield and failure behavior. See *DE- FINE_STOCHASTIC_VARIATION for additional information. *MAT_STEINBERG This is Material Type 11. This material is available for modeling materials deforming at very high strain rates (> 105) and can be used with solid elements. The yield strength is a function of temperature and pressure. An equation of state determines the pressure. Card 1 1 Variable MID 2 RO Type A8 F Card 2 Variable Type Card 3 Variable 1 B F 1 PC Type F Card 4 1 2 BP F 2 SPALL F 2 3 G0 F 3 H F 3 RP F 3 7 8 GAMA SIGM 4 5 SIGO BETA F 4 F F 4 F 5 A F 5 6 N F 6 F 7 TMO GAMO F 6 F 7 F 8 SA F 8 FLAG MMN MMX ECO EC1 F 4 F 5 F 6 F 7 F 8 Variable EC2 EC3 EC4 EC5 EC6 EC7 EC8 EC9 Type F F F F F F F F VARIABLE DESCRIPTION MID RO G0 Material identification. A unique number or label not exceeding 8 characters must be specified. Mass density. Basic shear modulus. VARIABLE DESCRIPTION SIGO BETA σo, see defining equations. β, see defining equations. N n, see defining equations. GAMA SIGM B BP H F A γi, initial plastic strain, see defining equations. σm, see defining equations. b, see defining equations. b′, see defining equations. h, see defining equations. f, see defining equations. Atomic weight (if = 0.0, R′ must be defined). TMO Tmo, see defining equations. GAMO γo, see defining equations. SA PC a, see defining equations. Pressure cutoff (default = -1.e+30) SPALL Spall type: EQ.0.0: default set to “2.0”, EQ.1.0: p ≥ PC, EQ.2.0: if σmax ≥ -PC element spalls and tension, p < 0, is never allowed, EQ.3.0: p < PC element spalls and tension, p < 0, is never allowed. R′. If R′≠0.0, A is not defined. Set to 1.0 for μ coefficients for the cold compression energy fit. Default is η. RP FLAG MMN μmin or ηmin. Optional μ or η minimum value. *MAT_STEINBERG DESCRIPTION MMX μmax or ηmax. Optional μ or η maximum value. EC0, …, EC9 Cold compression energy coefficients (optional). Remarks: Users who have an interest in this model are encouraged to study the paper by Steinberg and Guinan which provides the theoretical basis. Another useful reference is the KOVEC user’s manual. In terms of the foregoing input parameters, we define the shear modulus, 𝐺, before the material melts as: 𝐺 = 𝐺0 [1 + 𝑏𝑝𝑉 3⁄ − ℎ ( 𝐸𝑖 − 𝐸𝑐 3𝑅′ − 300)] 𝑒 −𝑓 𝐸𝑖 𝐸𝑚−𝐸𝑖 where 𝑝 is the pressure, 𝑉 is the relative volume, 𝐸𝑐 is the cold compression energy: 𝐸𝑐(𝑥) = ∫ 𝑝𝑑𝑥 − 900𝑅′exp(𝑎𝑥) (1 − 𝑥)2(𝛾0−𝑎−1 2⁄ ) , 𝑥 = 1 − 𝑉, and 𝐸𝑚 is the melting energy: which is in terms of the melting temperature 𝑇𝑚 (𝑥): 𝐸𝑚(𝑥) = 𝐸𝑐(𝑥) + 3𝑅′𝑇𝑚(𝑥) 𝑇𝑚(𝑥) = 𝑇𝑚𝑜exp(2𝑎𝑥) 𝑉2(𝛾𝑜−𝑎−1 3⁄ ) and the melting temperature at 𝜌 = 𝜌𝑜, 𝑇𝑚𝑜. In the above equation 𝑅′ is defined by 𝑅′ = 𝑅𝜌 where 𝑅 is the gas constant and A is the atomic weight. If 𝑅 is not defined, LS-DYNA computes it with 𝑅 in the cm-gram-microsecond system of units. The yield strength σy is given by: 𝜎𝑦 = 𝜎0 ′ [1 + 𝑏′𝑝𝑉 3⁄ − ℎ ( 𝐸𝑖 − 𝐸𝑐 3𝑅′ − 300)] 𝑒 −𝑓 𝐸𝑖 𝐸𝑚−𝐸𝑖 if 𝐸𝑚 exceeds 𝐸𝑖. Here, 𝜎0 ′ is given by: 𝜎0 ′ = 𝜎0[1 + 𝛽(𝛾𝑖 + 𝜀̅𝑝)]𝑛 where 0 is the initial yield stress and 𝑖 is the initial plastic strain. If the work-hardened is set equal to 𝑚. After the materials melt, 𝜎𝑦 and 𝐺 are yield stress 𝜎0 set to one half their initial value. ′ exceeds 𝑚, 𝜎0 ′ If the coefficients EC0, …, EC9 are not defined above, LS-DYNA will fit the cold compression energy to a ten term polynomial expansion either as a function of μ or η depending on the input variable, FLAG, as: 𝐸𝑐(𝜂𝑖) = ∑ 𝐸𝐶𝑖𝜂𝑖 𝑖=0 𝐸𝑐(𝜇𝑖) = ∑ 𝐸𝐶𝑖𝜇𝑖 𝑖=0 where ECi is the ith coefficient and: 𝜂 = 𝜌𝑜 𝜇 = 𝜌𝑜 − 1 A linear least squares method is used to perform the fit. A choice of three spall models is offered to represent material splitting, cracking, and failure under tensile loads. The pressure limit model, SPALL = 1, limits the hydrostatic tension to the specified value, pcut. If pressures more tensile than this limit are calculated, the pressure is reset to pcut. This option is not strictly a spall model, since the deviatoric stresses are unaffected by the pressure reaching the tensile cutoff, and the pressure cutoff value, pcut, remains unchanged throughout the analysis. The maximum principal stress spall model, SPALL = 2, detects spall if the maximum principal stress, σmax, exceeds the limiting value -pcut. Note that the negative sign is required because pcut is measured positive in compression, while σmax is positive in tension. Once spall is detected with this model, the deviatoric stresses are reset to zero, and no hydrostatic tension (p < 0) is permitted. If tensile pressures are calculated, they are reset to 0 in the spalled material. Thus, the spalled material behaves as a rubble or incohesive material. The hydrostatic tension spall model, SPALL = 3, detects spall if the pressure becomes more tensile than the specified limit, pcut. Once spall is detected the deviatoric stresses are reset to zero, and nonzero values of pressure are required to be compressive (positive). If hydrostatic tension (p < 0) is subsequently calculated, the pressure is reset to 0 for that element. This model is applicable to a wide range of materials, including those with pressure- dependent yield behavior. In addition, the incorporation of an equation of state permits accurate modeling of a variety of different materials. The spall model options permit incorporation of material failure, fracture, and disintegration effects under tensile loads. *MAT_STEINBERG_LUND This is Material Type 11. This material is a modification of the Steinberg model above to include the rate model of Steinberg and Lund [1989]. An equation of state determines the pressure. The keyword cards can appear in two ways: *MAT_STEINBERG_LUND or MAT_011_LUND Card 1 1 Variable MID 2 RO Type A8 F Card 2 Variable Type Card 3 Variable 1 B F 1 PC Type F Card 4 1 2 BP F 2 SPALL F 2 3 G0 F 3 H F 3 RP F 3 7 8 GAMA SIGM 4 5 SIGO BETA F 4 F F 4 F 5 A F 5 6 N F 6 F 7 TMO GAMO F 6 F 7 F 8 SA F 8 FLAG MMN MMX ECO EC1 F 4 F 5 F 6 F 7 F 8 Variable EC2 EC3 EC4 EC5 EC6 EC7 EC8 EC9 Type F F F F F F F Card 5 Variable 1 UK Type F 2 C1 F 3 C2 F 4 YP F 5 YA F 6 YM F 7 8 VARIABLE DESCRIPTION MID RO G0 SIGO BETA Material identification. A unique number or label not exceeding 8 characters must be specified. Mass density. Basic shear modulus. σo, see defining equations. β, see defining equations. N n, see defining equations. GAMA SIGM B BP H F A γi, initial plastic strain, see defining equations. σm, see defining equations. b, see defining equations. b′, see defining equations. h, see defining equations. f, see defining equations. Atomic weight (if = 0.0, R′ must be defined). TMO Tmo, see defining equations. GAMO γo, see defining equations. SA PC a, see defining equations. pcut or -σf (default = -1.e+30) VARIABLE DESCRIPTION SPALL Spall type: EQ.0.0: default set to “2.0”, EQ.1.0: p ≥ pmin, EQ.2.0: if 𝜎max ≥ −pmin element spalls and tension, p < 0, is never allowed, EQ.3.0: p < −pmin element spalls and tension, p < 0, is never allowed. R′. If R′≠0.0, A is not defined. Set to 1.0 for μ coefficients for the cold compression energy fit. Default is η. μmin or ηmin. Optional μ or η minimum value. μmax or ηmax. Optional μ or η maximum value. RP FLAG MMN MMX EC0, …, EC9 Cold compression energy coefficients (optional). UK C1 C2 YP YA Activation energy for rate dependent model. Exponent prefactor in rate dependent model. Coefficient of drag term in rate dependent model. Peierls stress for rate dependent model. A thermal yield stress for rate dependent model. YMAX Work hardening maximum for rate model. Remarks: This model is similar in theory to the *MAT_STEINBERG above but with the addition of rate effects. When rate effects are included, the yield stress is given by: 𝜎𝑦 = {𝑌𝑇(𝜀̇𝑝, 𝑇) + 𝑌𝐴𝑓 (𝜀𝑝)} 𝐺(𝑝, 𝑇) 𝐺0 There are two imposed limits on the yield stress. The first is on the thermal yield stress: 𝑌𝐴𝑓 (𝜀𝑝) = 𝑌𝐴[1 + 𝛽(𝛾𝑖 + 𝜀𝑝)]𝑛 ≤ 𝑌max and the second is on the thermal part: 𝑌𝑇 ≤ 𝑌𝑃 R' is the heat capacity per unit volume. Most handbooks give the heat capacity per unit mass or per mole. To obtain R', multiply the heat capacity per unit mass by the initial density, and to obtain R' from the heat capacity per mole, divide it by the mass per mole and then multiply the result by the initial density. The mass per mole in grams equals the atomic weight. For example, the heat capacity per mole for aluminum is 24.2 J/mole/K, the density is 2.70 g/cc, and the atomic weight is 13. The heat capacity per cubic centimeter is therefore (24.2 J/mole/K) / (13g/mole) × (2.70g/cc)= 5.026 J/cc/K. To convert it to J/m3/K, multiply the result by 106 cc/m3 to obtain a final heat capacity of 5.026e6 J/m3/K. *MAT_ISOTROPIC_ELASTIC_PLASTIC This is Material Type 12. This is a very low cost isotropic plasticity model for three- dimensional solids. In the plane stress implementation for shell elements, a one-step radial return approach is used to scale the Cauchy stress tensor to if the state of stress exceeds the yield surface. This approach to plasticity leads to inaccurate shell thickness updates and stresses after yielding. This is the only model in LS-DYNA for plane stress that does not default to an iterative approach. Card 1 Variable MID 2 RO Type A8 F 3 G F 4 5 6 7 8 SIGY ETAN BULK F F F VARIABLE DESCRIPTION MID RO G SIGY ETAN BULK Material identification. A unique number or label not exceeding 8 characters must be specified. Mass density. Shear modulus. Yield stress. Plastic hardening modulus. Bulk modulus, K. Remarks: Here the pressure is integrated in time where 𝜀̇𝑖𝑖 is the volumetric strain rate. 𝑝̇ = −𝐾𝜀̇𝑖𝑖 *MAT_ISOTROPIC_ELASTIC_FAILURE This is Material Type 13. This is a non-iterative plasticity with simple plastic strain failure model. Card 1 1 Variable MID 2 RO Type A8 F 3 G F 4 5 6 7 8 SIGY ETAN BULK F F F Default none none none none 0.0 none Card 2 1 2 3 4 5 6 7 8 Variable EPF PRF REM TREM Type F F F F Default none 0.0 0.0 0.0 VARIABLE DESCRIPTION MID RO G SIGY ETAN BULK EPF PRF Material identification. A unique number or label not exceeding 8 characters must be specified. Mass density. Shear modulus. Yield stress. Plastic hardening modulus. Bulk modulus. Plastic failure strain. Failure pressure (≤ 0.0). *MAT_ISOTROPIC_ELASTIC_FAILURE DESCRIPTION REM Element erosion option: EQ.0.0: failed element eroded after failure, NE.0.0: element is kept, no removal except by Δt below. TREM Δt for element removal: EQ.0.0: Δt is not considered (default), GT.0.0: element eroded if element time step size falls below Δt. Remarks: When the effective plastic strain reaches the failure strain or when the pressure reaches the failure pressure, the element loses its ability to carry tension and the deviatoric stresses are set to zero, i.e., the material behaves like a fluid. If Δt for element removal is defined the element removal option is ignored. The element erosion option based on Δt must be used cautiously with the contact options. Nodes to surface contact is recommended with all nodes of the eroded brick elements included in the node list. As the elements are eroded the mass remains and continues to interact with the master surface. *MAT_SOIL_AND_FOAM_FAILURE This is Material Type 14. The input for this model is the same as for *MATERIAL_- SOIL_AND_FOAM (Type 5); however, when the pressure reaches the tensile failure pressure, the element loses its ability to carry tension. It should be used only in situations when soils and foams are confined within a structure or are otherwise confined by nodal boundary conditions. *MAT_JOHNSON_COOK_{OPTION} Available options include: <BLANK> STOCHASTIC This is Material Type 15. The Johnson/Cook strain and temperature sensitive plasticity is sometimes used for problems where the strain rates vary over a large range and adiabatic temperature increases due to plastic heating cause material softening. When used with solid elements this model requires an equation-of-state. If thermal effects and damage are unimportant, the much less expensive *MAT_SIMPLIFIED_JOHN- SON_COOK model is recommended. The simplified model can be used with beam elements. Card 1 1 Variable MID 2 RO Type A8 F 3 G F 4 E F 5 PR F 6 DTF F 7 VP F 8 RATEOP F Default none none none none none 0.0 0.0 0.0 Card 2 Variable Type 1 A F 2 B F 3 N F 4 C F 5 M F 6 TM F 7 TR F 8 EPS0 F Default none 0.0 0.0 0.0 none none none none Card 3 Variable 1 CP Type F 2 PC F 3 SPALL F 4 IT F 5 D1 F 6 D2 F 7 D3 F 8 D4 F Default none 0.0 2.0 0.0 0.0 0.0 0.0 0.0 Card 4 1 2 3 4 5 6 7 8 Variable D5 C2/P/XNP EROD EFMIN NUMINT Type F F F F Default 0.0 0.0 0.0 10-6 F 0. VARIABLE DESCRIPTION MID RO G E PR DTF Material identification. A unique number or label not exceeding 8 characters must be specified. Mass density Shear modulus. G and an equation-of-state are required for element types that use a 3D stress update, e.g., solids, 2D shell forms 13-15, tshell forms 3 and 5. For other element types, G is ignored, and E and PR must be provided. Young’s Modulus . Poisson’s ratio . Minimum time step size for automatic element deletion (shell elements). The element will be deleted when the solution time step size drops below DTF × TSSFAC where TSSFAC is the time step scale factor defined by *CONTROL_TIMESTEP. VP Formulation for rate effects: EQ.0.0: Scale yield stress (default), EQ.1.0: Viscoplastic formulation. *MAT_JOHNSON_COOK DESCRIPTION RATEOP Form of strain-rate term. RATEOP is ignored if VP = 0. EQ.0.0: Log-Linear Johnson-Cook (default), EQ.1.0: Log-Quadratic Huh-Kang (2 parameters), EQ.2.0: Exponential Allen-Rule-Jones, EQ.3.0: Exponential Cowper-Symonds (2 parameters). EQ.4.0: Nonlinear rate coefficient (2 parameters). A B N C M TM TR EPS0 CP PC See equations below See equations below See equations below See equations below See equations below Melt temperature Room temperature Quasi-static threshold strain rate. Ideally, this value represents the highest strain rate for which no rate adjustment to the flow stress is needed, and is input in units of [time]−1. For example, if strain rate effects on the flow stress first become apparent at strain rates greater than 10−2s−1 and the system of units for the model input is kg, mm, ms, then EPSO should be set to 10−5, which is 10−2s−1 in units of ms. Specific heat (superseded by heat capacity in *MAT_THER- MAL_OPTION if a coupled thermal/structural analysis) Tensile failure stress or tensile pressure cutoff (PC < 0.0) VARIABLE DESCRIPTION SPALL Spall type: EQ.0.0: default set to “2.0”. EQ.1.0: Tensile pressure is limited by PC, i.e., 𝑝 is always ≥ PC. Shell Element Specific Behavior: EQ.2.0: Shell elements are deleted when 𝜎max ≥ −PC. EQ.3.0: Shell elements are deleted when 𝑝 < 𝑃𝐶. Solid Element Specific Behavior EQ.2.0: For solid elements 𝜎max ≥ −PC resets tensile stresses to zero. Compressive stress are still allowed. EQ.3.0: For solid elements 𝑝 < PC resets the pressure to zero thereby disallowing tensile pressure. IT Plastic strain iteration option. This input applies to solid elements only since it is always necessary to iterate for the shell element plane stress condition. EQ.0.0: no iterations (default), EQ.1.0: accurate iterative solution for plastic strain. Much more expensive than default. D1 - D5 Failure parameters, see equations below. A negative input of D3 will be converted to its absolute value. C2/P/XNP Optional strain-rate parameter. Field Var Model C2 P XNP 𝐶2 Huh-Kang 𝑃 Cowper-Symonds 𝑛′ Nonlinear Rate Coefficient These models are documented in the remarks. EROD Erosion Flag: EQ.0.0: default, element erosion allowed. NE.0.0: element does not erode; deviatoric stresses set to zero when element fails. EFMIN The lower bound for calculated strain at fracture . NUMINT *MAT_JOHNSON_COOK DESCRIPTION Number of through thickness integration points which must fail before the shell element is deleted. (If zero, all points must fail.) Since nodal fiber rotations limit strains at active integration points, the default, which is to require that all integration points fail, is not recommended, because elements undergoing large strain are often not deleted using this criterion. Better results may be obtained when NUMINT is set to 1 or a number less than one half of the number of through thickness points. For example, if four through thickness points are used, NUMINT should not exceed 2, even for fully integrated shells which have 16 integration points. Remarks: Johnson and Cook express the flow stress as 𝜎𝑦 = (𝐴 + 𝐵𝜀̅𝑝𝑛 )(1 + 𝑐 ln 𝜀̇∗)(1 − 𝑇∗𝑚) Where, 𝐴, 𝐵, 𝑐, 𝑛, and 𝑚 = input constants 𝜀̅𝑝 = effective plastic strain 𝜀̇∗ = ⎧ ε̅ {{ ⎨ {{ ⎩ EPS0 ̇𝑝 ε̅ EPS0 for VP.EQ.0 (normalized effective total strain-rate) for VP.EQ. 1 (normalized effective plastic strain rate) 𝑇∗ = homologous temperature = 𝑇 − 𝑇room 𝑇melt − 𝑇room The quantity 𝑇 − 𝑇room is stored as extra history variable 5. Constants for a variety of materials are provided in Johnson and Cook [1983]. A fully viscoplastic formulation is optional (VP) which incorporates the rate equations within the yield surface. An additional cost is incurred but the improvement is that results can be dramatic. Due to nonlinearity in the dependence of flow stress on plastic strain, an accurate value of the flow stress requires iteration for the increment in plastic strain. However, by using a Taylor series expansion with linearization about the current time, we can solve for σy with sufficient accuracy to avoid iteration. 2-136 (EOS) *MAT_015 𝜀𝑓 = max([𝐷1 + 𝐷2exp𝐷3𝜎 ∗][1 + 𝐷4ln𝜀̇∗][1 + 𝐷5𝑇∗], EFMIN) where σ* is the ratio of pressure divided by effective stress Fracture occurs when the damage parameter 𝜎 ∗ = 𝜎eff 𝐷 = ∑ Δ𝜀𝑝 𝜀𝑓 reaches the value of 1. 𝐷 is stored as extra history variable 4 in shell elements and extra history variable 6 in solid elements. A choice of three spall models is offered to represent material splitting, cracking, and failure under tensile loads. The pressure limit model limits the minimum hydrostatic pressure to the specified value, 𝑝 ≥ 𝑝min. If pressures more tensile than this limit are calculated, the pressure is reset to 𝑝min. This option is not strictly a spall model since the deviatoric stresses are unaffected by the pressure reaching the tensile cutoff and the pressure cutoff value 𝑝min remains unchanged throughout the analysis. The maximum principal stress spall model detects spall if the maximum principal stress, 𝜎max, exceeds the limiting value 𝜎𝑝. Once spall in solids is detected with this model, the deviatoric stresses are reset to zero and no hydrostatic tension is permitted. If tensile pressures are calculated, they are reset to 0 in the spalled material. Thus, the spalled material behaves as rubble. The hydrostatic tension spall model detects spall if the pressure becomes more tensile than the specified limit, 𝑝min. Once spall in solids is detected with this model, the deviatoric stresses are set to zero and the pressure is required to be compressive. If hydrostatic tension is calculated then the pressure is reset to 0 for that element. In addition to the above failure criterion, this material model also supports a shell element deletion criterion based on the maximum stable time step size for the element, Δ𝑡max. Generally, Δ𝑡max goes down as the element becomes more distorted. To assure stability of time integration, the global LS-DYNA time step is the minimum of the Δ𝑡max values calculated for all elements in the model. Using this option allows the selective deletion of elements whose time step Δ𝑡max has fallen below the specified minimum time step, Δ𝑡crit. Elements which are severely distorted often indicate that material has failed and supports little load, but these same elements may have very small time steps and therefore control the cost of the analysis. This option allows these highly distorted elements to be deleted from the calculation, and, therefore, the analysis can proceed at a larger time step, and, thus, at a reduced cost. Deleted elements do not carry any load, and are deleted from all applicable slide surface definitions. Clearly, this option must be judiciously used to obtain accurate results at a minimum cost. Material type 15 is applicable to the high rate deformation of many materials including most metals. Unlike the Steinberg-Guinan model, the Johnson-Cook model remains valid down to lower strain rates and even into the quasistatic regime. Typical applications include explosive metal forming, ballistic penetration, and impact. Optional Strain Rate Forms: The standard Johnson-Cook strain rate term is linear in the logarithm of the strain rate: 1 + 𝐶 ln 𝜀̇∗ Some additional data fitting capability can be obtained by using the quadratic form proposed by Huh & Kang [2002]: 1 + 𝐶 ln 𝜀̇∗ + 𝐶2(ln 𝜀̇∗)2 Three additional exponential forms are available, one due to Allen, Rule & Jones [1997], (𝜀̇∗)𝑐 the Cowper-Symonds-like [1958] form and the nonlinear rate coefficient, 𝜀̇eff ⎟⎞ 𝐶 ⎠ ⎜⎛ ⎝ 1 + 𝑛′ 𝑝 ) 1 + 𝐶(𝜀eff ln 𝜀̇∗. The four additional rate forms (RATEOP = 1, 2, 3 or 4) are currently available for solid & shell elements but only when the viscoplastic rate option is active (VP = 1). If VP is set to zero, RATEOP is ignored. See Huh and Kang [2002], Allen, Rule, and Jones [1997], and Cowper and Symonds [1958]. The STOCHASTIC option allows spatially varying yield and failure behavior. See *DE- FINE_STOCHASTIC_VARIATION for additional information. *MAT_016 This is Material Type 16. This model has been used to analyze buried steel reinforced concrete structures subjected to impulsive loadings. 5 6 7 8 Card 1 1 Variable MID 2 RO Type A8 F 3 G F 4 PR F Default none none none none Card 2 1 Variable SIGF Type F 2 A0 F 3 A1 F 4 A2 F 5 6 A0F A1F F F 7 B1 F 8 PER F Default 0.0 0.0 0.0 0.0 0.0 0.0 0.0 0.0 Card 3 Variable 1 ER 2 3 4 5 6 7 8 PRR SIGY ETAN LCP LCR Type F F F F F F Default 0.0 0.0 none 0.0 none none Variable 1 X1 Type F *MAT_PSEUDO_TENSOR 2 X2 F 3 X3 F 4 X4 F 5 X5 F 6 X6 F 7 X7 F 8 X8 F Default none none none none none none none none Card 5 Variable 1 X9 2 3 4 5 6 7 8 X10 X11 X12 X13 X14 X15 X16 Type F F F F F F F F Default none none none none none none none none Card 6 1 2 3 4 5 6 7 8 Variable YS1 YS2 YS3 YS4 YS5 YS6 YS7 YS8 Type F F F F F F F F Default none none none none none none none none Card 7 1 2 3 4 5 6 7 8 Variable YS9 YS10 YS11 YS12 YS13 YS14 YS15 YS16 Type F F F F F F F F Default none none none none none none none none VARIABLE DESCRIPTION MID RO G PR Material identification. A unique number or label not exceeding 8 characters must be specified. Mass density. Shear modulus. Poisson’s ratio. SIGF Tensile cutoff (maximum principal stress for failure). A0 A1 A2 A0F A1F B1 PER ER PRR SIGY ETAN LCP LCR Xn Cohesion. Pressure hardening coefficient. Pressure hardening coefficient. Cohesion for failed material. Pressure hardening coefficient for failed material. Damage scaling factor (or exponent in Mode II.C). Percent reinforcement. Elastic modulus for reinforcement. Poisson’s ratio for reinforcement. Initial yield stress. Tangent modulus/plastic hardening modulus. Load curve ID giving rate sensitivity for principal material, see *DEFINE_CURVE. Load curve ID giving rate sensitivity for reinforcement, see *DE- FINE_CURVE. Effective plastic strain, damage, or pressure. See discussion below. YSn Yield stress (Mode I) or scale factor (Mode II.B or II.C). Mohr-Coulomb Tresca Friction Angle Cohesion Figure M16-1. Mohr-Coulomb surface with a Tresca Limit. Pressure Remarks: This model can be used in two major modes - a simple tabular pressure-dependent yield surface, and a potentially complex model featuring two yield versus pressure functions with the means of migrating from one curve to the other. For both modes, load curve LCP is taken to be a strain rate multiplier for the yield strength. Note that this model must be used with equation-of-state type 8, 9 or 11. Response Mode I. Tabulated Yield Stress Versus Pressure This model is well suited for implementing standard geologic models like the Mohr- Coulomb yield surface with a Tresca limit, as shown in Figure M16-1. Examples of converting conventional triaxial compression data to this type of model are found in (Desai and Siriwardane, 1984). Note that under conventional triaxial compression conditions, the LS-DYNA input corresponds to an ordinate of 𝜎1 − 𝜎3 rather than the more widely used , where 𝜎1 is the maximum principal stress and 𝜎3is the minimum principal stress. 𝜎1−𝜎3 This material combined with equation-of-state type 9 (saturated) has been used very successfully to model ground shocks and soil-structure interactions at pressures up to 100kbars (approximately 1.5 x 106 psi). Figure M16-2. Two-curve concrete model with damage and failure Pressure To invoke Mode I of this model, set a0, a1, a2, b1, a0f, and a1f to zero. The tabulated values of pressure should then be specified on cards 4 and 5, and the corresponding values of yield stress should be specified on cards 6 and 7. The parameters relating to reinforcement properties, initial yield stress, and tangent modulus are not used in this response mode, and should be set to zero. Simple tensile failure Note that a1f is reset internally to 1/3 even though it is input as zero; this defines a failed material curve of slope 3p, where p denotes pressure (positive in compression). In this case the yield strength is taken from the tabulated yield vs. pressure curve until the maximum principal stress (𝜎1) in the element exceeds the tensile cutoff 𝜎cut (input as variable SIGF). When 𝜎1 > 𝜎cut is detected, the yield strength is scaled back by a fraction of the distance between the two curves in each of the next 20 time steps so that after those 20 time steps, the yield strength is defined by the failure curve. The only way to inhibit this feature is to set 𝜎𝑐𝑢𝑡 (SIGF) arbitrarily large. Response Mode II. Two Curve Model with Damage and Failure This approach uses two yield versus pressure curves of the form 𝜎𝑦 = 𝑎0 + 𝑎1 + 𝑎2𝑝 The upper curve is best described as the maximum yield strength curve and the lower curve is the failed material curve. There are a variety of ways of moving between the two curves and each is discussed below. MODE II. A: Simple tensile failure Define a0, a1, a2, a0f and a1f, set b1 to zero, and leave cards 4 through 7 blank. In this case the yield strength is taken from the maximum yield curve until the maximum principal stress (𝜎1) in the element exceeds the tensile cutoff (𝜎cut). When 𝜎1 > 𝜎cut is detected, the yield strength is scaled back by a fraction of the distance between the two curves in each of the next 20 time steps so that after those 20 time steps, the yield strength is defined by the failure curve. Mode II.B: Tensile failure plus plastic strain scaling Define a0, a1, a2, a0f and a1f, set b1 to zero, and user cards 4 through 7 to define a scale factor, η, versus effective plastic strain. LS-DYNA evaluates η at the current effective plastic strain and then calculated the yield stress as 𝜎yield = 𝜎failed + 𝜂(𝜎max − 𝜎failed) where 𝜎max and 𝜎failed are found as shown in Figure M16-2. This yield strength is then subject to scaling for tensile failure as described above. This type of model allows the description of a strain hardening or softening material such as concrete. Mode II.C: Tensile failure plus damage scaling The change in yield stress as a function of plastic strain arises from the physical mechanisms such as internal cracking, and the extent of this cracking is affected by the hydrostatic pressure when the cracking occurs. This mechanism gives rise to the "confinement" effect on concrete behavior. To account for this phenomenon, a "damage" function was defined and incorporated. This damage function is given the form: 𝜀𝑝 𝜆 = ∫ (1 + 𝜎cut ) −𝑏1 𝑑𝜀𝑝 Define a0, a1, a2, a0f and a1f, and b1. Cards 4 though 7 now give η as a function of λ and scale the yield stress as and then apply any tensile failure criteria. 𝜎yield = 𝜎failed + 𝜂(𝜎max − 𝜎failed) Mode II Concrete Model Options Material Type 16 Mode II provides for the automatic internal generation of a simple "generic" model from concrete if A0 is negative then SIGF is assumed to be the ′ and –A0 is assumed to be a conversion unconfined concrete compressive strength, 𝑓𝑐 factor from LS-DYNA pressure units to psi. (For example, if the model stress units are MPa, A0 should be set to –145.) In this case the parameter values generated internally are ′ = SIGF 𝑓𝑐 𝜎𝑐𝑢𝑡 = 1.7 ′2 ⎜⎛ 𝑓𝑐 ⎟⎞ −𝐴0⎠ ⎝ 𝑎0 = ′ 𝑓𝑐 𝑎1 = 𝑎2 = ′ 3𝑓𝑐 𝑎0𝑓 = 0 𝑎1𝑓 = 0.385 Note that these a0f and a1f defaults will be overridden by non zero entries on Card 3. If plastic strain or damage scaling is desired, Cards 5 through 8 and b1 should be specified in the input. When a0 is input as a negative quantity, the equation-of-state can be given as 0 and a trilinear EOS Type 8 model will be automatically generated from the unconfined compressive strength and Poisson's ratio. The EOS 8 model is a simple pressure versus volumetric strain model with no internal energy terms, and should give reasonable results for pressures up to 5kbar (approximately 75,000 psi). Mixture model A reinforcement fraction, 𝑓𝑟, can be defined (indirectly as PER/100) along with properties of the reinforcement material. The bulk modulus, shear modulus, and yield strength are then calculated from a simple mixture rule, i.e., for the bulk modulus the rule gives: 𝐾 = (1 − 𝑓𝑟)𝐾𝑚 + 𝑓𝑟𝐾𝑟 where 𝐾𝑚 and 𝐾𝑟 are the bulk moduli for the geologic material and the reinforcement material, respectively. This feature should be used with caution. It gives an isotropic effect in the material instead of the true anisotropic material behavior. A reasonable approach would be to use the mixture elements only where the reinforcing exists and plain elements elsewhere. When the mixture model is being used, the strain rate multiplier for the principal material is taken from load curve N1 and the multiplier for the reinforcement is taken from load curve N2. A Suggestion The LLNL DYNA3D manual from 1991 [Whirley and Hallquist] suggests using the damage function (Mode II.C.) in Material Type 16 with the following set of parameters: 𝑎0 = 𝑎1 = ′ 𝑓𝑐 𝑎2 = 𝑎0𝑓 = ′ 3𝑓𝑐 ′ 𝑓𝑐 10 𝑎1𝑓 = 1.5 𝑏1 = 1.25 *MAT_PSEUDO_TENSOR Card 4: Card 5: Card 6: Card 7: 0.0 5.17E-04 8.62E-06 6.38E-04 2.15E-05 7.98E-04 3.14E-05 3.95E-04 9.67E-04 4.00E-03 1.41E-03 4.79E-03 1.97E-03 0.909 2.59E-03 3.27E-03 0.309 0.790 0.383 0.086 0.543 0.630 0.247 0.056 0.840 0.469 0.173 0.0 0.975 1.000 0.136 0.114 This set of parameters should give results consistent with Dilger, Koch, and Kowalczyk, [1984] for plane concrete. It has been successfully used for reinforced structures where the reinforcing bars were modeled explicitly with embedded beam and shell elements. The model does not incorporate the major failure mechanism - separation of the concrete and reinforcement leading to catastrophic loss of confinement pressure. However, experience indicates that this physical behavior will occur when this model shows about 4% strain. *MAT_017 This is Material Type 17. This material may be used to model brittle materials which fail due to large tensile stresses. Card 1 1 Variable MID 2 RO Type A8 F 3 E F 4 PR F 5 6 SIGY ETAN F F 7 FS F 8 PRF F Default none none none none none 0.0 none 0.0 Optional card for crack propagation to adjacent elements : Card 2 1 2 3 4 5 6 7 8 Variable SOFT CVELO Type F F Default 1.0 0.0 VARIABLE DESCRIPTION MID RO E PR SIGY ETAN FS PRF Material identification. A unique number or label not exceeding 8 characters must be specified. Mass density. Young’s modulus. Poisson’s ratio. Yield stress. Plastic hardening modulus. Fracture stress. Failure or cutoff pressure (≤ 0.0). SOFT *MAT_ORIENTED_CRACK DESCRIPTION Factor by which the fracture stress is reduced when a crack is coming from failed neighboring element. See remarks. CVELO Crack propagation velocity. See remarks. Remarks: This is an isotropic elastic-plastic material which includes a failure model with an oriented crack. The von Mises yield condition is given by: 𝜙 = 𝐽2 − 𝜎𝑦 where the second stress invariant, 𝐽2, is defined in terms of the deviatoric stress components as 𝐽2 = 𝑠𝑖𝑗𝑠𝑖𝑗 and the yield stress,𝜎𝑦, is a function of the effective plastic strain, 𝜀eff hardening modulus, 𝐸𝑝: 𝑝 , and the plastic The effective plastic strain is defined as: 𝑝 𝜎𝑦 = 𝜎0 + 𝐸𝑝𝜀eff 𝑝 = ∫ 𝑑𝜀eff 𝜀eff where 𝑝 = √ 𝑑𝜀eff 𝑝 𝑝 𝑑𝜀𝑖𝑗 𝑑𝜀𝑖𝑗 and the plastic tangent modulus is defined in terms of the input tangent modulus, 𝐸𝑡, as 𝐸𝑝 = 𝐸𝐸𝑡 𝐸 − 𝐸𝑡 Pressure in this model is found from evaluating an equation of state. A pressure cutoff can be defined such that the pressure is not allowed to fall below the cutoff value. The oriented crack fracture model is based on a maximum principal stress criterion. When the maximum principal stress exceeds the fracture stress, 𝜎𝑓 , the element fails on a plane perpendicular to the direction of the maximum principal stress. The normal stress and the two shear stresses on that plane are then reduced to zero. This stress reduction is done according to a delay function that reduces the stresses gradually to zero over a small number of time steps. This delay function procedure is used to reduce Figure M17-1. Thin structure (2 elements over thickness) with cracks and necessary element numbering. the ringing that may otherwise be introduced into the system by the sudden fracture. The number of steps for stress reduction is 20 by default (CVELO = 0.0) or it is internally computed if CVELO > 0.0 is given: where Le is characteristic element length and Δt is time step size. 𝑛steps = int [ 𝐿𝑒 CVELO × 𝛥𝑡 ] After a tensile fracture, the element will not support tensile stress on the fracture plane, but in compression will support both normal and shear stresses. The orientation of this fracture surface is tracked throughout the deformation, and is updated to properly model finite deformation effects. If the maximum principal stress subsequently exceeds the fracture stress in another direction, the element fails isotropically. In this case the element completely loses its ability to support any shear stress or hydrostatic tension, and only compressive hydrostatic stress states are possible. Thus, once isotropic failure has occurred, the material behaves like a fluid. This model is applicable to elastic or elastoplastic materials under significant tensile or shear loading when fracture is expected. Potential applications include brittle materials such as ceramics as well as porous materials such as concrete in cases where pressure hardening effects are not significant. Crack propagation behavior to adjacent elements can be controlled via parameter SOFT for thin, shell-like structures (e.g. only 2 or 3 solids over thickness). Additionally, LS- DYNA has to know where the plane or solid element midplane is at each integration point for projection of crack plane on this element midplane. Therefore, element numbering has to be as shown in Figure M17-1. Only solid element type 1 is supported with that option at the moment. *MAT_POWER_LAW_PLASTICITY This is Material Type 18. This is an isotropic plasticity model with rate effects which uses a power law hardening rule. Card 1 1 Variable MID 2 RO Type A8 F 3 E F 4 PR F 5 K F 6 N F 7 8 SRC SRP F F Default none none none none none none 0.0 0.0 Card 2 1 Variable SIGY Type F 2 VP F 3 4 5 6 7 8 EPSF F Default 0.0 0.0 0.0 VARIABLE DESCRIPTION MID RO E PR K N SRC SRP Material identification. A unique number or label not exceeding 8 characters must be specified. Mass density. Young’s modulus. Poisson’s ratio. Strength coefficient. Hardening exponent. Strain rate parameter, 𝐶, if zero, rate effects are ignored. Strain rate parameter, 𝑃, if zero, rate effects are ignored. VARIABLE SIGY DESCRIPTION Optional input parameter for defining the initial yield stress, 𝜎𝑦. Generally, this parameter is not necessary and the strain to yield is calculated as described below. LT.0.02: 𝜀𝑦𝑝 = SIGY GT.0.02: See below. Plastic failure strain for element deletion. Formulation for rate effects: EQ.0.0: Scale yield stress (default), EQ.1.0: Viscoplastic formulation. EPSF VP Remarks: Elastoplastic behavior with isotropic hardening is provided by this model. The yield stress, 𝜎𝑦, is a function of plastic strain and obeys the equation: 𝜎𝑦 = 𝑘𝜀𝑛 = 𝑘(𝜀𝑦𝑝 + 𝜀̅𝑝) where 𝜀𝑦𝑝 is the elastic strain to yield and 𝜀̅𝑝is the effective plastic strain (logarithmic). If SIGY is set to zero, the strain to yield if found by solving for the intersection of the linearly elastic loading equation with the strain hardening equation: 𝜎 = 𝐸𝜀 𝜎 = 𝑘 𝜀𝑛 which gives the elastic strain at yield as: If SIGY is nonzero and greater than 0.02 then: 𝜀𝑦𝑝 = ( [ 1 ] 𝑛−1 ) 𝜀𝑦𝑝 = ( [1 𝑛] ) 𝜎𝑦 Strain rate is accounted for using the Cowper and Symonds model which scales the yield stress with the factor 1 + ( 𝑝⁄ ) 𝜀̇ where 𝜀̇ is the strain rate. A fully viscoplastic formulation is optional which incorporates the Cowper and Symonds formulation within the yield surface. An additional cost is incurred but the improvement is results can be dramatic. *MAT_STRAIN_RATE_DEPENDENT_PLASTICITY This is Material Type 19. A strain rate dependent material can be defined. For an alternative, see Material Type 24. Required is a curve for the yield stress versus the effective strain rate. Optionally, Young’s modulus and the tangent modulus can also be defined versus the effective strain rate. Also, optional failure of the material can be defined either by defining a von Mises stress at failure as a function of the effective strain rate (valid for solids/shells/thick shells) or by defining a minimum time step size (only for shells). Card 1 1 Variable MID 2 RO Type A8 F 3 E F 4 PR F 5 VP F Default none none none none 0.0 6 7 8 Card 2 1 2 3 4 5 6 7 8 Variable LC1 ETAN LC2 LC3 LC4 TDEL RDEF Type F F F F F F F Default none 0.0 0.0 0.0 0.0 0.0 0.0 VARIABLE DESCRIPTION MID RO E PR VP Material identification. A unique number or label not exceeding 8 characters must be specified. Mass density. Young’s modulus. Poisson’s ratio. Formulation for rate effects: EQ.0.0: Scale yield stress (default), EQ.1.0: Viscoplastic formulation LC1 ETAN LC2 LC3 LC4 TDEL *MAT_STRAIN_RATE_DEPENDENT_PLASTICITY DESCRIPTION Load curve ID defining the yield stress σ0 as a function of the effective strain rate. Tangent modulus, Et Load curve ID defining Young’s modulus as a function of the effective (available only when VP = 0; not strain recommended). rate Load curve ID defining tangent modulus as a function of the effective strain rate (optional). Load curve ID defining von Mises stress at failure as a function of the effective strain rate (optional). Minimum time step size for automatic element deletion. Use for shells only. RDEF Redefinition of failure curve: EQ.1.0: Effective plastic strain, EQ.2.0: Maximum principal stress and absolute value of minimum principal stress, EQ.3.0: Maximum principal stress (release 5 of v.971) Remarks: In this model, a load curve is used to describe the yield strength 𝜎0 as a function of effective strain rate 𝜀̅ ̇ where 𝜀̅ ̇ = ( 2⁄ ′ ) ′ 𝜀̇𝑖𝑗 𝜀̇𝑖𝑗 and the prime denotes the deviatoric component. The strain rate is available for post- processing as the first stored history variable. If the viscoplastic option is active, the plastic strain rate is output; otherwise, the effective strain rate defined above is output. The yield stress is defined as 𝜎𝑦 = 𝜎0(𝜀̅ ̇) + 𝐸𝑝𝜀̅𝑝 where 𝜀̅𝑝 is the effective plastic strain and 𝐸𝑝 is given in terms of Young’s modulus and the tangent modulus by 𝐸𝑝 = 𝐸𝐸𝑡 𝐸 − 𝐸𝑡 . Both Young's modulus and the tangent modulus may optionally be made functions of strain rate by specifying a load curve ID giving their values as a function of strain rate. If these load curve ID's are input as 0, then the constant values specified in the input are used. Note that all load curves used to define quantities as a function of strain rate must have the same number of points at the same strain rate values. This requirement is used to allow vectorized interpolation to enhance the execution speed of this constitutive model. This model also contains a simple mechanism for modeling material failure. This option is activated by specifying a load curve ID defining the effective stress at failure as a function of strain rate. For solid elements, once the effective stress exceeds the failure stress the element is deemed to have failed and is removed from the solution. For shell elements the entire shell element is deemed to have failed if all integration points through the thickness have an effective stress that exceeds the failure stress. After failure the shell element is removed from the solution. In addition to the above failure criterion, this material model also supports a shell element deletion criterion based on the maximum stable time step size for the element, Δ𝑡max. Generally, Δ𝑡max goes down as the element becomes more distorted. To assure stability of time integration, the global LS-DYNA time step is the minimum of the Δ𝑡max values calculated for all elements in the model. Using this option allows the selective deletion of elements whose time step Δ𝑡max has fallen below the specified minimum time step, Δ𝑡crit. Elements which are severely distorted often indicate that material has failed and supports little load, but these same elements may have very small time steps and therefore control the cost of the analysis. This option allows these highly distorted elements to be deleted from the calculation, and, therefore, the analysis can proceed at a larger time step, and, thus, at a reduced cost. Deleted elements do not carry any load, and are deleted from all applicable slide surface definitions. Clearly, this option must be judiciously used to obtain accurate results at a minimum cost. A fully viscoplastic formulation is optional which incorporates the rate formulation within the yield surface. An additional cost is incurred but the improvement is results can be dramatic. *MAT_RIGID This is Material 20. Parts made from this material are considered to belong to a rigid body (for each part ID). Also, the coupling of a rigid body with MADYMO and CAL3D can be defined via this material. Alternatively, a VDA surface can be attached as surface to model the geometry, e.g., for the tooling in metalforming applications. Also, global and local constraints on the mass center can be optionally defined. Optionally, a local consideration for output and user-defined airbag sensors can be chosen. 5 N F 0 5 Card 1 1 2 Variable MID RO Type A8 F 3 E F 4 PR F Default none none none none Card 2 1 2 3 4 Variable CMO CON1 CON2 Type Default F 0 F 0 F 0 Optional for output (Must be included but may be left blank). Card 3 1 2 Variable LCO or A1 A2 Type Default F 0 F 0 3 A3 F 0 4 V1 F 0 5 V2 F 0 7 M F 0 7 8 ALIAS or RE C/F blank none 8 7 8 6 COUPLE F 0 6 6 V3 F MID RO E PR N *MAT_020 DESCRIPTION Material identification. A unique number or label not exceeding 8 characters must be specified. Mass density Young’s modulus. Reasonable values have to be chosen for contact analysis (choice of penalty), see Remarks below. Poisson’s ratio. Reasonable values have to be chosen for contact analysis (choice of penalty), see Remarks below. MADYMO3D 5.4 coupling flag, n: EQ.0: use normal LS-DYNA rigid body updates, GT.0: the rigid body is coupled to MADYMO 5.4 ellipsoid number n LT.0: the rigid body is coupled to MADYMO 5.4 plane number |n|. COUPLE Coupling option if applicable: EQ.-1: attach VDA surface in ALIAS (defined in the eighth field) and automatically generate a mesh for viewing the surface in LS-PREPOST. MADYMO 5.4 / CAL3D coupling option: EQ.0: the undeformed geometry to LS-DYNA corresponds to the local system for MADYMO 5.4 / CAL3D. The finite element mesh is input, input EQ.1: the undeformed geometry to LS-DYNA corresponds to the global system for MADYMO 5.4 / CAL3D, input EQ.2: generate a mesh for the ellipsoids and planes internally in LS-DYNA. M MADYMO3D 5.4 coupling flag, m: EQ.0: use normal LS-DYNA rigid body updates, EQ.m: this rigid body corresponds to MADYMO rigid body number m. Rigid body updates are performed by MADYMO. ALIAS VDA surface alias name, see Appendix L. RE CMO DESCRIPTION MADYMO 6.0.1 External Reference Number Center of mass constraint option, CMO: EQ.+1.0: constraints applied in global directions, EQ.0.0: no constraints, *MAT_RIGID EQ.-1.0: constraints constraint). applied in local directions (SPC CON1 First constraint parameter: If CMO = +1.0, then specify global translational constraint: EQ.0: no constraints, EQ.1: constrained x displacement, EQ.2: constrained y displacement, EQ.3: constrained z displacement, EQ.4: constrained x and y displacements, EQ.5: constrained y and z displacements, EQ.6: constrained z and x displacements, EQ.7: constrained x, y, and z displacements. If CM0 = -1.0, then specify local coordinate system ID. See *DEFINE_COORDINATE_OPTION: This coordinate system is fixed in time. CON2 Second constraint parameter: If CMO = +1.0, then specify global rotational constraint: EQ.0: no constraints, EQ.1: constrained x rotation, EQ.2: constrained y rotation, EQ.3: constrained z rotation, EQ.4: constrained x and y rotations, EQ.5: constrained y and z rotations, EQ.6: constrained z and x rotations, EQ.7: constrained x, y, and z rotations. VARIABLE DESCRIPTION If CM0 = -1.0, then specify local (SPC) constraint: EQ.000000: no constraint, EQ.100000: constrained x translation, EQ.010000: constrained y translation, EQ.001000: constrained z translation, EQ.000100: constrained x rotation, EQ.000010: constrained y rotation, EQ.000001: constrained z rotation. Any combination of local constraints can be achieved by adding the number 1 into the corresponding column. LCO Local coordinate system number for output. A1 - V3 Alternative method for specifying local system below: Define two vectors a and v, fixed in the rigid body which are used for output and the user defined airbag sensor subrou- tines. The output parameters are in the directions a, b, and c where the latter are given by the cross products c = a × v and b = c × a. This input is optional. Remarks: The rigid material type 20 provides a convenient way of turning one or more parts comprised of beams, shells, or solid elements into a rigid body. Approximating a deformable body as rigid is a preferred modeling technique in many real world applications. For example, in sheet metal forming problems the tooling can properly and accurately be treated as rigid. In the design of restraint systems the occupant can, for the purposes of early design studies, also be treated as rigid. Elements which are rigid are bypassed in the element processing and no storage is allocated for storing history variables; consequently, the rigid material type is very cost efficient. Two unique rigid part ID's may not share common nodes unless they are merged together using the rigid body merge option. A rigid body may be made up of disjoint finite element meshes, however. LS-DYNA assumes this is the case since this is a common practice in setting up tooling meshes in forming problems. All elements which reference a given part ID corresponding to the rigid material should be contiguous, but this is not a requirement. If two disjoint groups of elements on opposite sides of a model are modeled as rigid, separate part ID's should be created for each of the contiguous element groups if each group is to move independently. This requirement arises from the fact that LS-DYNA internally computes the six rigid body degrees-of-freedom for each rigid body (rigid material or set of merged materials), and if disjoint groups of rigid elements use the same part ID, the disjoint groups will move together as one rigid body. Inertial properties for rigid materials may be defined in either of two ways. By default, the inertial properties are calculated from the geometry of the constituent elements of the rigid material and the density specified for the part ID. Alternatively, the inertial properties and initial velocities for a rigid body may be directly defined, and this overrides data calculated from the material property definition and nodal initial velocity definitions. Young's modulus, E, and Poisson's ratio, υ are used for determining sliding interface parameters if the rigid body interacts in a contact definition. Realistic values for these constants should be defined since unrealistic values may contribute to numerical problem in contact. Constraint directions for rigid materials (CMO equal to +1 or -1) are fixed, that is, not updated, with time. To impose a constraint on a rigid body such that the constraint direction is updated as the rigid body rotates, use *BOUNDARY_PRESCRIBED_MO- TION_RIGID_LOCAL. It is strongly advised that nodal constraints, e.g., by *BOUNDARY_SPC_OPTION, not be applied to nodes of a rigid body as doing so may compromise the intended constraints in the case of an explicit simulation. Such SPCs will be skipped in an implicit simulation and a warning issued. If the intended constraints are not with respect to the calculated center-of-mass of the rigid body, *CONSTRAINED_JOINT_OPTION may often be used to obtain the desired effect. This approach typically entails defining a second rigid body which is fully constrained and then defining a joint between the two rigid bodies. Another alternative for defining rigid body constraints that are not with respect to the calculated center-of- mass of the rigid body is to manually specify the initial center-of-mass location using *PART_INERTIA. When using *PART_INERTIA, a full set of mass properties must be specified and the user must understand that the dynamic behavior of the rigid body is affected by its mass properties. For coupling with MADYMO 5.4.1, only basic coupling is available. The coupling flags (N and M) must match with SYSTEM and ELLIP- SOID/PLANE in the MADYMO input file and the coupling option (COUPLE) must be defined. For coupling with MADYMO 6.0.1, both basic and extended coupling are available: 1. Basic Coupling: The external reference number (RE) must match with the external reference number in the MADYMO XML input file. The coupling option (COUPLE) must be defined. 2. Extended Coupling: Under this option MADYMO will handle the contact between the MADYMO and LS-DYNA models. The external reference number (RE) and the coupling option (COUPLE) are not needed. All coupling surfaces that interface with the MADYMO models need to be defined in *CONTACT_- COUPLING. *MAT_ORTHOTROPIC_THERMAL_{OPTION} This is Material Type 21. A linearly elastic, orthotropic material with orthotropic thermal expansion. Available options include: <BLANK> FAILURE CURING Card 1 1 Variable MID Type A8 Card 2 1 2 RO F 2 3 EA F 3 Variable GAB GBC GCA Type F F F Card 3 Variable 1 XP Type F Card 4 Variable 1 V1 Type F 2 YP F 2 V2 F 3 ZP F 3 V3 F 4 EB F 4 AA F 4 A1 F 4 D1 F 5 EC F 5 AB F 5 A2 F 5 D2 F 6 7 8 PRBA PRCA PRCB F 6 AC F 6 A3 F 6 D3 F F 7 F 8 AOPT MACF F 7 I 8 7 8 BETA REF Required for failure. Card 5 Variable 1 A1 2 A11 Type F F 3 A2 F Additional card 5 required for curing. Card 5 Variable 1 K1 Type F 2 K2 F 3 C1 F Additional card 6 required for curing. 4 A5 F 4 C2 F 5 A55 F 5 M F 6 A4 F 6 N F 7 NIP F 7 R F 8 8 Card 6 1 2 3 4 5 6 7 8 Variable LCCHA LCCHB LCCHC LCAA LCAB LCAC Type I I I I I I VARIABLE DESCRIPTION MID RO EA EB EC PRBA PRCA PRCB Material identification. A unique number or label not exceeding 8 characters must be specified. Mass density. 𝐸𝑎, Young’s modulus in 𝑎-direction. 𝐸𝑏, Young’s modulus in 𝑏-direction. 𝐸𝑐, Young’s modulus in 𝑐-direction. 𝜈𝑏𝑎, Poisson’s ratio, 𝑏𝑎. 𝜈𝑐𝑎, Poisson’s ratio, 𝑐𝑎. 𝜈𝑐𝑏, Poisson’s ratio, 𝑐𝑏 *MAT_ORTHOTROPIC_THERMAL DESCRIPTION GAB GBC GCA AA AB AC AOPT 𝐺𝑎𝑏, Shear modulus, 𝑎𝑏. 𝐺𝑏𝑐, Shear modulus, 𝑏𝑐. 𝐺𝑐𝑎, Shear modulus, 𝑐𝑎. 𝛼𝑎, coefficient of thermal expansion in the 𝑎-direction. 𝛼𝑏, coefficient of thermal expansion in the 𝑏-direction. 𝛼𝑐, coefficient of thermal expansion in the 𝑐-direction. Material axes option : EQ.0.0: locally orthotropic with material axes determined by element nodes 1, 2, and 4, as with *DEFINE_COORDI- NATE_NODES, and then, for shells only, rotated about the shell element normal by an angle BETA. EQ.1.0: locally orthotropic with material axes determined by a point in space and the global location of the element center; this is the a-direction. This option is for solid elements only. EQ.2.0: globally orthotropic with material axes determined by vectors defined below, as with *DEFINE_COORDI- NATE_VECTOR. EQ.3.0: locally orthotropic material axes determined by rotating the material axes about the element normal by an angle, BETA, from a line in the plane of the element defined by the cross product of the vector v with the element normal. EQ.4.0: locally orthotropic in cylindrical coordinate system with the material axes determined by a vector 𝐯, and an originating point, 𝐩, which define the centerline ax- is. This option is for solid elements only. LT.0.0: the absolute value of AOPT is a coordinate system ID number (CID on *DEFINE_COORDINATE_NODES, *DEFINE_COORDINATE_SYSTEM or *DEFINE_CO- ORDINATE_VECTOR). Available in R3 version of 971 and later. VARIABLE DESCRIPTION MACF Material axes change flag for brick elements: EQ.1: No change, default, EQ.2: switch material axes a and b, EQ.3: switch material axes a and c, EQ.4: switch material axes b and c. XP, YP, ZP Coordinates of point 𝐩 for AOPT = 1 and 4. A1, A2, A3 Components of vector 𝐚 for AOPT = 2. V1, V2, V3 Components of vector 𝐯 for AOPT = 3 and 4. D1, D2, D3 Components of vector 𝐝 for AOPT = 2. BETA REF Material angle in degrees for AOPT = 1 (shells only) and AOPT = 3, may be overridden on the element card, see *ELE- MENT_SHELL_BETA or *ELEMENT_SOLID_ORTHO. Use reference geometry to initialize the stress tensor. The reference geometry is defined by the keyword:*INITIAL_FOAM_- REFERENCE_GEOMETRY . EQ.0.0: off, EQ.1.0: on. A1, A11, A2 A5, A55, A4 Coefficients for the matrix dominated failure criterion. Coefficients for the fiber dominated failure criterion. K1 K2 C1 C2 M N R Parameter 𝑘1 for Kamal model. For details see remark below. Parameter 𝑘2 for Kamal model. Parameter 𝑐1 for Kamal model. Parameter 𝑐2 for Kamal model. Exponent 𝑚 for Kamal model. Exponent 𝑛 for Kamal model. Gas constant for Kamal model. LCCHA LCCHB LCCHC LCAA *MAT_ORTHOTROPIC_THERMAL DESCRIPTION Load curve for 𝛾𝑎, coefficient of chemical shrinkage in the 𝑎- direction. Input 𝛾𝑎 as function of state of cure 𝛽. Load curve for 𝛾𝑏, coefficient of chemical shrinkage in the 𝑏- direction. Input 𝛾𝑏 as function of state of cure 𝛽. Load curve for 𝛾𝑐, coefficient of chemical shrinkage in the 𝑐- direction. Input 𝛾𝑐 as function of state of cure 𝛽. Load curve or table ID for 𝛼𝑎. If defined parameter AA is ignored. IF LCID Input 𝛼𝑎 versus temperature. IF TABID: Input 𝛼𝑎 as functions of state of cure (table values) and temperatures Load curve ID for 𝛼𝑏. If defined parameter AB is ignored. See LCAA for further details. Load curve ID for 𝛼𝑐. If defined parameter AC is ignored. See LCAA for further details. LCAB LCAC Remarks: In the implementation for three-dimensional continua a total Lagrangian formulation is used. In this approach the material law that relates second Piola-Kirchhoff stress 𝐒 to the Green-St. Venant strain 𝐄 is where 𝐓 is the transformation matrix [Cook 1974]. 𝐒 = 𝐂 ⋅ 𝐄 = 𝐓T𝐂𝑙𝐓 ⋅ 𝐄 𝐓 = 𝑙1 𝑙2 𝑙3 2𝑙1𝑙2 2𝑙2𝑙3 2𝑙3𝑙1 ⎡ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎣ 𝑚1 𝑚2 𝑚3 2𝑚1𝑚2 2𝑚2𝑚3 2𝑚3𝑚1 𝑛1 𝑛2 𝑚3 2𝑛1𝑛2 2𝑛2𝑛3 2𝑛3𝑛1 𝑙1𝑚1 𝑙2𝑚2 𝑙3𝑚3 (𝑙1𝑚2 + 𝑙2𝑚1) (𝑙2𝑚3 + 𝑙3𝑚2) (𝑙3𝑚1 + 𝑙1𝑚3) 𝑚1𝑛1 𝑚2𝑛2 𝑚3𝑛3 (𝑚1𝑛2 + 𝑚2𝑛1) (𝑚2𝑛3 + 𝑚3𝑛2) (𝑚3𝑛1 + 𝑚1𝑛3) 𝑛1𝑙1 ⎤ ⎥ 𝑛2𝑙2 ⎥ ⎥ 𝑛3𝑙3 ⎥ ⎥ (𝑛1𝑙2 + 𝑛2𝑙1) ⎥ (𝑛2𝑙3 + 𝑛3𝑙2) ⎥ (𝑛3𝑙1 + 𝑛1𝑙3)⎦ 𝑙𝑖, 𝑚𝑖, 𝑛𝑖 are the direction cosines ′ = 𝑙𝑖𝑥1 + 𝑚𝑖𝑥2 + 𝑛𝑖𝑥3 for 𝑖 = 1, 2, 3 𝑥𝑖 ′ denotes the material axes. The constitutive matrix 𝐂𝑙 is defined in terms of the and 𝑥𝑖 material axes as −1 = 𝐂𝑙 𝐸11 𝜐12 𝐸11 𝜐13 𝐸11 − − − 𝜐21 𝐸22 𝐸22 𝜐23 𝐸22 − − − 𝜐31 𝐸33 𝜐32 𝐸33 𝐸33 ⎡ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎣ 𝐺12 𝐺23 ⎤ ⎥ ⎥ ⎥ ⎥ ⎥ ⎥ ⎥ ⎥ ⎥ ⎥ ⎥ ⎥ ⎥ ⎥ ⎥ ⎥ 𝐺31 ⎦ where the subscripts denote the material axes, i.e., ′ ′ and 𝐸𝑖𝑖 = 𝐸𝑥𝑖 𝜐𝑖𝑗 = 𝜐𝑥𝑖 ′𝑥𝑗 Since 𝐂𝑙 is symmetric 𝜐12 𝐸11 = 𝜐21 𝐸22 , … The vector of Green-St. Venant strain components is 𝐄T = [𝐸11, 𝐸22, 𝐸33, 𝐸12, 𝐸23, 𝐸31] which include the local thermal strains which are integrated in time: 𝑛+1 = 𝜀𝑎𝑎 𝜀𝑎𝑎 𝑛+1 = 𝜀𝑏𝑏 𝜀𝑏𝑏 𝑛+1 = 𝜀𝑐𝑐 𝜀𝑐𝑐 𝑛 + 𝛼𝑎(𝑇𝑛+1 − 𝑇𝑛) 𝑛 + 𝛼𝑏(𝑇𝑛+1 − 𝑇𝑛) 𝑛 + 𝛼𝑐(𝑇𝑛+1 − 𝑇𝑛) where 𝑇 is temperature. After computing 𝑆𝑖𝑗 we then obtain the Cauchy stress: 𝜎𝑖𝑗 = 𝜌0 ∂𝑥𝑖 ∂𝑋𝑘 ∂𝑥𝑗 ∂𝑋𝑙 𝑆𝑘𝑙 This model will predict realistic behavior for finite displacement and rotations as long as the strains are small. In the implementation for shell elements, the stresses are integrated in time and are updated in the corotational coordinate system. In this procedure the local material axes are assumed to remain orthogonal in the deformed configuration. This assumption is valid if the strains remain small. The failure models were derived by William Feng. The first one defines the matrix dominated failure mode, 𝐹𝑚 = 𝐴1(𝐼1 − 3) + 𝐴11(𝐼1 − 3)2 + 𝐴2(𝐼2 − 3) − 1 and the second defines the fiber dominated failure mode, 𝐹𝑓 = 𝐴5(𝐼5 − 1) + 𝐴55(𝐼5 − 1)2 + 𝐴4(𝐼4 − 1) − 1. When either is greater than zero, the integration point fails, and the element is deleted after NIP integration points fail. The coefficients 𝐴𝑖 are defined in the input and the invariants 𝐼𝑖 are the strain invariants 𝐼1 = ∑ 𝐶𝛼𝛼 𝛼=1,3 𝐼2 = [𝐼1 2 − ∑ 𝐶𝛼𝛽 𝛼,𝛽=1,3 ] 𝐼3 = det(𝐂) 𝐼4 = ∑ 𝑉𝛼 𝛼,𝛽,𝛾=1,3 𝐶𝛼𝛾𝐶𝛾𝛽𝑉𝛽 𝐼5 = ∑ 𝑉𝛼 𝛼,𝛽=1,3 𝐶𝛼𝛽𝑉𝛽 and 𝐂 is the Cauchy strain tensor and 𝐕 is the fiber direction in the undeformed state. By convention in this material model, the fiber direction is aligned with the 𝑎 direction of the local orthotropic coordinate system. The curing option implies that orthotropic chemical shrinkage is to be considered, resulting from a curing process in the material. The state of cure 𝛽 is an internal material variable that follows the Kamal model = (𝐾1 + 𝐾2𝛽𝑚)(1 − 𝛽)𝑛 with 𝐾1 = 𝑘1𝑒 − 𝑐1 𝑅𝑇, 𝐾2 = 𝑘2𝑒 − 𝑐2 𝑅𝑇 𝑑𝛽 𝑑𝑡 and chemical strains are introduced: 𝑛+1 = 𝜀𝑎𝑎 𝜀𝑎𝑎 𝑛+1 = 𝜀𝑏𝑏 𝜀𝑏𝑏 𝑛+1 = 𝜀𝑐𝑐 𝜀𝑐𝑐 𝑛 + 𝛾𝑎(𝛽𝑛+1 − 𝛽𝑛) 𝑛 + 𝛾𝑏(𝛽𝑛+1 − 𝛽𝑛) 𝑛 + 𝛾𝑐(𝛽𝑛+1 − 𝛽𝑛) The coefficients 𝛾𝑎, 𝛾𝑏, 𝛾𝑐 can be defined as functions of the state of cure 𝛽. Furthermore, the coefficients of thermal expansion 𝛼𝑎, 𝛼𝑏, 𝛼𝑐can also be defined as functions of the state of cure 𝛽 and the temperature 𝑇, if the curing option is used. *MAT_022 This is Material Type 22. An orthotropic material with optional brittle failure for composites can be defined following the suggestion of [Chang and Chang 1987a, 1987b]. Three failure criteria are possible, see the LS-DYNA Theory Manual. By using the user defined integration rule, see *INTEGRATION_SHELL, the constitutive constants can vary through the shell thickness. For all shells, except the DKT formulation, laminated shell theory can be activated to properly model the transverse shear deformation. Lamination theory is applied to correct for the assumption of a uniform constant shear strain through the thickness of the shell. For sandwich shells where the outer layers are much stiffer than the inner layers, the response will tend to be too stiff unless lamination theory is used. To turn on lamination theory see *CONTROL_SHELL. Card 1 1 Variable MID 2 RO Type A8 F 3 EA F 4 EB F 5 EC F 6 7 8 PRBA PRCA PRCB F F F Default none none none none none none none none Card 2 1 2 3 4 5 6 7 8 Variable GAB GBC GCA KFAIL AOPT MACF ATRACK Type F F F F F Default none none none 0.0 0.0 I 0 I Variable 1 XP Type F *MAT_COMPOSITE_DAMAGE 2 YP F 3 ZP F 4 A1 F 5 A2 F 6 A3 F 7 8 Default 0.0 0.0 0.0 0.0 0.0 0.0 Card 4 Variable 1 V1 Type F 2 V2 F 3 V3 F 4 D1 F 5 D2 F 6 D3 F 7 8 BETA F Default 0.0 0.0 0.0 0.0 0.0 0.0 0.0 Card 5 Variable 1 SC Type F 2 XT F 3 YT F 4 YC F 5 ALPH F 6 SN F 7 8 SYZ SZX F F Default none none none none none none none none VARIABLE DESCRIPTION MID RO EA EB EC Material identification. A unique number or label not exceeding 8 characters must be specified. Mass density 𝐸𝑎, Young’s modulus in 𝑎-direction. 𝐸𝑏, Young’s modulus in 𝑏-direction. 𝐸𝑐, Young’s modulus in 𝑐-direction. PRBA 𝜈𝑏𝑎, Poisson ratio, 𝑏𝑎. VARIABLE DESCRIPTION PRCA PRCB GAB GBC GCA KFAIL AOPT 𝜈𝑐𝑎, Poisson ratio, 𝑐𝑎. 𝜈𝑐𝑏, Poisson ratio, 𝑐𝑏. 𝐺𝑎𝑏, Shear modulus, 𝑎𝑏. 𝐺𝑏𝑐, Shear modulus, 𝑏𝑐. 𝐺𝑐𝑎, Shear modulus, 𝑐𝑎. Bulk modulus of failed material. Necessary for compressive failure. Material axes option : EQ.0.0: locally orthotropic with material axes determined by element nodes 1, 2, and 4, as with *DEFINE_COORDI- NATE_NODES, and then, for shells only, rotated about the shell element normal by an angle BETA. EQ.1.0: locally orthotropic with material axes determined by a point in space and the global location of the element center; this is the 𝑎-direction. This option is for solid elements only. EQ.2.0: globally orthotropic with material axes determined by vectors defined below, as with *DEFINE_COORDI- NATE_VECTOR. EQ.3.0: locally orthotropic material axes determined by rotating the material axes about the element normal by an angle, BETA, from a line in the plane of the element defined by the cross product of the vector v with the element normal. EQ.4.0: locally orthotropic in cylindrical coordinate system with the material axes determined by a vector 𝐯, and an originating point, 𝐩, which define the centerline ax- is. This option is for solid elements only. LT.0.0: the absolute value of AOPT is a coordinate system ID number (CID on *DEFINE_COORDINATE_NODES, *DEFINE_COORDINATE_SYSTEM or *DEFINE_CO- ORDINATE_VECTOR). Available in R3 version of 971 and later. *MAT_COMPOSITE_DAMAGE DESCRIPTION MACF Material axes change flag for brick elements: EQ.1: No change, default, EQ.2: switch material axes 𝑎 and 𝑏, EQ.3: switch material axes 𝑎 and 𝑐, EQ.4: switch material axes 𝑏 and 𝑐. ATRACK Material a-axis tracking flag (shell elements only) EQ.0: a-axis rotates with element (default) EQ.1: a-axis also tracks deformation XP, YP, ZP Coordinates of point 𝐩 for AOPT = 1 and 4. A1, A2, A3 Components of vector 𝐚 for AOPT = 2. V1, V2, V3 Components of vector 𝐯 for AOPT = 3 and 4. D1, D2, D3 Components of vector 𝐝 for AOPT = 2. Material angle in degrees for AOPT = 0 (shells only) and AOPT = 3, may be overridden on the element card, see *ELE- MENT_SHELL_BETA or *ELEMENT_SOLID_ORTHO. Shear strength, ab plane, see the LS-DYNA Theory Manual. Longitudinal tensile strength, 𝑎-axis, see the LS-DYNA Theory Manual. Transverse tensile strength, 𝑏-axis. Transverse compressive strength, 𝑏-axis (positive value). Shear stress parameter for the nonlinear term, see the LS-DYNA Theory Manual. Suggested range 0 – 0.5. Normal tensile strength (solid elements only) Transverse shear strength (solid elements only) Transverse shear strength (solid elements only) BETA SC XT YT YC ALPH SN SYZ SZX Remarks: 1. History Data. The number of additional integration point variables for shells written to the d3plot database is specified using the *DATABASE_EXTENT_BI- NARY keyword on the NEIPS field. These additional history variables are enumerated below: History Variable3 Description Value ef(𝑖) tensile fiber mode LS-PrePost history variable See below table cm(𝑖) ed(𝑖) tensile matrix mode compressive mode matrix 1 - elastic 0 - failed 1 2 The following components are stored as element component 7 instead of the effective plastic strain. Note that ef(𝑖) for 𝑖 = 1,2,3 is not retrievable. Description Integration point nip nip ∑ ef(𝑖) 𝑖=1 nip nip ∑ cm(𝑖) 𝑖=1 nip nip ∑ ed(𝑖) 𝑖=1 ef(𝑖) for 𝑖 > 3 1 2 3 𝑖 2. The ATRACK Field. The initial material directions are set using AOPT and the related data. By default, the material directions in shell elements are updated each cycle based on the rotation of the 1-2 edge, or else the rotation of all edges if the invariant node numbering option is set on *CONTROL_ACCURACY. When ATRACK=1, an optional scheme is used in which the 𝑎-direction of the material tracks element deformation as well as rotation. At the start of the calculation, a line is passed through each element center in the direction of the material a-axis. This line will intersect the edges of the element at two points. The referential coordinates of these two points are stored, and then used throughout the calculation to locate these points in the deformed geometry. The material 𝑎-axis is assumed to be in the direction of the line that passes through both points. If ATRACK = 0, the layers of a layered 3 (cid:1861) ranges over the shell integration points. composite will always rotate together. However, if ATRACK = 1, the layers can rotate independently which may be more accurate, particularly for shear de- formation. This option is available only for shell elements. *MAT_TEMPERATURE_DEPENDENT_ORTHOTROPIC This is Material Type 23. An orthotropic elastic material with arbitrary temperature dependency can be defined. Card 1 1 Variable MID 2 RO 3 4 5 6 7 8 AOPT REF MACF Type A8 F F F I Card 2 Variable 1 XP Type F Card 3 Variable 1 V1 Type F 2 YP F 2 V2 F 3 ZP F 3 V3 F 4 A1 F 4 D1 F 5 A2 F 5 D2 F 6 A3 F 6 D3 F 7 8 7 8 BETA F Temperature Card Pairs. Define one set of constants on two cards using formats 4 and 5 for each temperature point. Up to 48 points (96 cards) can be defined. The next “*” card terminates the input. First Temperature Card. Card 4 1 Variable EAi 2 EBi 3 4 5 6 7 8 ECi PRBAi PRCAi PRCBi Type F F F F F Second Temperature Card Card 5 1 Variable AAi 2 ABi 3 4 5 6 ACi GABi GBCi GCAi Type F F F F F F 8 7 Ti F VARIABLE MID DESCRIPTION Material identification. A unique number or label not exceeding 8 characters must be specified. RO Mass density. AOPT Material axes option : EQ.0.0: locally orthotropic with material axes determined by element nodes 1, 2, and 4, as with *DEFINE_COORDI- NATE_NODES, and then, for shells only, rotated about the shell element normal by an angle BETA. EQ.1.0: locally orthotropic with material axes determined by a point in space and the global location of the element center; this is the 𝑎-direction. This option is for solid elements only. EQ.2.0: globally orthotropic with material axes determined by vectors defined below, as with *DEFINE_COORDI- NATE_VECTOR. EQ.3.0: locally orthotropic material axes determined by rotating the material axes about the element normal by an angle, BETA, from a line in the plane of the element defined by the cross product of the vector 𝐯 with the element normal. EQ.4.0: locally orthotropic in cylindrical coordinate system with the material axes determined by a vector 𝐯, and an originating point, 𝐩, which define the centerline ax- is. This option is for solid elements only. LT.0.0: the absolute value of AOPT is a coordinate system ID number (CID on *DEFINE_COORDINATE_NODES, *DEFINE_COORDINATE_SYSTEM or *DEFINE_CO- ORDINATE_VECTOR). Available in R3 version of 971 VARIABLE DESCRIPTION and later. REF Use reference geometry to initialize the stress tensor. The reference geometry is defined by the keyword:*INITIAL_FOAM_- REFERENCE_GEOMETRY . EQ.0.0: off, EQ.1.0: on. MACF Material axes change flag for brick elements: EQ.1: No change, default, EQ.2: switch material axes 𝑎 and 𝑏, EQ.3: switch material axes 𝑎 and 𝑐, EQ.4: switch material axes 𝑏 and 𝑐. XP, YP, ZP Coordinates of point 𝐩 for AOPT = 1 and 4. A1, A2, A3 Components of vector 𝐚 for AOPT = 2. V1, V2, V3 Components of vector 𝐯 for AOPT = 3 and 4. D1, D2, D3 Components of vector 𝐝 for AOPT = 2. BETA EAi EBi ECi PRBAi PRCAi PRCBi AAi ABi Material angle in degrees for AOPT = 0 (shells only) and AOPT = 3, may be overridden on the element card, see *ELE- MENT_SHELL_BETA or *ELEMENT_SOLID_ORTHO. 𝐸𝑎, Young’s modulus in 𝑎-direction at temperature Ti. 𝐸𝑏, Young’s modulus in 𝑏-direction at temperature Ti. 𝐸𝑐, Young’s modulus in 𝑐-direction at temperature Ti. 𝜈𝑏𝑎, Poisson’s ratio 𝑏𝑎 at temperature Ti. 𝜈𝑐𝑎, Poisson’s ratio 𝑐𝑎 at temperature Ti. 𝜈𝑐𝑏, Poisson’s ratio 𝑐𝑏 at temperature Ti. 𝛼𝑎, coefficient of thermal expansion in 𝑎-direction at temperature Ti. 𝛼𝐵 coefficient of thermal expansion in 𝑏-direction at temperature Ti. 𝛼𝑐, coefficient of thermal expansion in 𝑐-direction at temperature Ti. 𝐺𝑎𝑏, Shear modulus 𝑎𝑏 at temperature Ti. 𝐺𝑏𝑐, Shear modulus 𝑏𝑐 at temperature Ti. 𝐺𝑐𝑎, Shear modulus 𝑐𝑎 at temperature Ti. ith temperature *MAT_023 VARIABLE ACi GABi GBCi GCAi Ti Remarks: In the implementation for three-dimensional continua a total Lagrangian formulation is used. In this approach the material law that relates second Piola-Kirchhoff stress 𝐒 to the Green-St. Venant strain 𝐄 is where 𝐓 is the transformation matrix [Cook 1974]. 𝐒 = 𝐂 ⋅ 𝐄 = 𝐓T𝐂𝒍𝐓 ⋅ 𝐄 𝐓 = 𝑙1 𝑙2 𝑙3 2𝑙1𝑙2 2𝑙2𝑙3 2𝑙3𝑙1 ⎡ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎣ 𝑚1 𝑚2 𝑚3 2𝑚1𝑚2 2𝑚2𝑚3 2𝑚3𝑚1 𝑛1 𝑛2 𝑚3 2𝑛1𝑛2 2𝑛2𝑛3 2𝑛3𝑛1 𝑙1𝑚1 𝑙2𝑚2 𝑙3𝑚3 (𝑙1𝑚2 + 𝑙2𝑚1) (𝑙2𝑚3 + 𝑙3𝑚2) (𝑙3𝑚1 + 𝑙1𝑚3) 𝑚1𝑛1 𝑚2𝑛2 𝑚3𝑛3 (𝑚1𝑛2 + 𝑚2𝑛1) (𝑚2𝑛3 + 𝑚3𝑛2) (𝑚3𝑛1 + 𝑚1𝑛3) 𝑛1𝑙1 ⎤ ⎥ 𝑛2𝑙2 ⎥ ⎥ 𝑛3𝑙3 ⎥ ⎥ (𝑛1𝑙2 + 𝑛2𝑙1) ⎥ (𝑛2𝑙3 + 𝑛3𝑙2) ⎥ (𝑛3𝑙1 + 𝑛1𝑙3)⎦ 𝑙𝑖, 𝑚𝑖, 𝑛𝑖 are the direction cosines ′ = 𝑙𝑖𝑥1 + 𝑚𝑖𝑥2 + 𝑛𝑖𝑥3 for 𝑖 = 1, 2, 3 𝑥𝑖 ′ denotes the material axes. The temperature dependent constitutive matrix 𝐂𝑙 is and 𝑥𝑖 defined in terms of the material axes as 𝐸11(𝑇) 𝜐12(𝑇) 𝐸11(𝑇) 𝜐13(𝑇) 𝐸11(𝑇) − − − 𝜐21(𝑇) 𝐸22(𝑇) 𝐸22(𝑇) 𝜐23(𝑇) 𝐸22(𝑇) − − − 𝜐31(𝑇) 𝐸33(𝑇) 𝜐32(𝑇) 𝐸33(𝑇) 𝐸33(𝑇) −1 = 𝐂𝑙 ⎡ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎣ 𝐺12(𝑇) 𝐺23(𝑇) ⎤ ⎥ ⎥ ⎥ ⎥ ⎥ ⎥ ⎥ ⎥ ⎥ ⎥ ⎥ ⎥ ⎥ ⎥ ⎥ ⎥ 𝐺31(𝑇) ⎦ where the subscripts denote the material axes, i.e., ′ ′ and 𝐸𝑖𝑖 = 𝐸𝑥𝑖 𝜐𝑖𝑗 = 𝜐𝑥𝑖 ′𝑥𝑗 Since 𝐂𝑙 is symmetric 𝜐12 𝐸11 = 𝜐21 𝐸22 , … The vector of Green-St. Venant strain components is 𝐄T = ⌊𝐸11, 𝐸22, 𝐸33, 𝐸12, 𝐸23, 𝐸31⌋ which include the local thermal strains which are integrated in time: 𝑛+1 = 𝜀𝑎𝑎 𝜀𝑎𝑎 𝑛 + 𝛼𝑎 (𝑇 𝑛+1 2) [𝑇𝑛+1 − 𝑇𝑛] 𝑛+1 = 𝜀𝑏𝑏 𝜀𝑏𝑏 𝑛 + 𝛼𝑏 (𝑇 𝑛+1 2) [𝑇𝑛+1 − 𝑇𝑛] 𝑛+1 = 𝜀𝑐𝑐 𝜀𝑐𝑐 𝑛 + 𝛼𝑐 (𝑇 𝑛+1 2) [𝑇𝑛+1 − 𝑇𝑛] where 𝑇 is temperature. After computing 𝑆𝑖𝑗 we then obtain the Cauchy stress: 𝜎𝑖𝑗 = 𝜌0 ∂𝑥𝑖 ∂𝑋𝑘 ∂𝑥𝑗 ∂𝑋𝑙 𝑆𝑘𝑙 This model will predict realistic behavior for finite displacement and rotations as long as the strains are small. For shell elements, the stresses are integrated in time and are updated in the corotational coordinate system. In this procedure the local material axes are assumed to remain orthogonal in the deformed configuration. This assumption is valid if the strains remain small. *MAT_PIECEWISE_LINEAR_PLASTICITY_{OPTION} Available options include: <BLANK> LOG_INTERPOLATION STOCHASTIC MIDFAIL This is Material Type 24, which is an elasto-plastic material with an arbitrary stress versus strain curve and arbitrary strain rate dependency can be defined. See also Remark below. Also, failure based on a plastic strain or a minimum time step size can be defined. For another model with a more comprehensive failure criteria see MAT_ MODIFIED_PIECEWISE_LINEAR_PLASTICITY. If considering laminated or sandwich shells with non-uniform material properties (this is defined through the user specified integration rule), the model, MAT_LAYERED_LINEAR_PLASTICITY, is recommended. If solid elements are used and if the elastic strains before yielding are finite, the model, MAT_FINITE_ELASTIC_STRAIN_PLASTICITY, treats the elastic strains using a hyperelastic formulation. The LOG_INTERPOLATION option interpolates the strain rate effect in table LCSS with logarithmic interpolation. The STOCHASTIC option allows spatially varying yield and failure behavior. See *DE- FINE_STOCHASTIC_VARIATION for additional information. The MIDFAIL option is available only for shell elements. When included on the keyword line, this option causes failure to be checked only at the mid-plane of the element. If an element has an even number of layers, failure is checked in the two layers closest to the mid-plane. Card 1 1 Variable MID 2 RO Type A8 F 3 E F 4 PR F 5 6 7 8 SIGY ETAN FAIL TDEL F F F Default none none none none none 0.0 1021 F Card 2 Variable Type Default 1 C F 0 Card 3 1 2 P F 0 2 3 4 LCSS LCSR F 0 3 F 0 4 5 VP F 0 5 6 7 8 6 7 8 Variable EPS1 EPS2 EPS3 EPS4 EPS5 EPS6 EPS7 EPS8 Type Default F 0 Card 4 1 F 0 2 F 0 3 F 0 4 F 0 5 F 0 6 F 0 7 F 0 8 Variable ES1 ES2 ES3 ES4 ES5 ES6 ES7 ES8 Type Default F 0 F 0 F 0 F 0 F 0 F 0 F 0 F 0 VARIABLE DESCRIPTION MID RO E PR Material identification. A unique number or label not exceeding 8 characters must be specified. Mass density. Young’s modulus. Poisson’s ratio. SIGY Yield stress. Figure M24-1. Rate effects may be accounted for by defining a table of curves. If a table ID is specified a curve ID is given for each strain rate, see *DEFINE_TABLE. Intermediate values are found by interpolating between curves. Effective plastic strain versus yield stress is expected. If the strain rate values fall out of range, extrapolation is not used; rather, either the first or last curve determines the yield stress depending on whether the rate is low or high, respectively. VARIABLE DESCRIPTION ETAN Tangent modulus, ignored if (LCSS.GT.0) is defined. FAIL Failure flag. LT.0.0: User defined failure subroutine, matusr_24 in dyn21.F, is called to determine failure EQ.0.0: Failure is not considered. This option is recommended if failure is not of interest since many calculations will be saved. GT.0.0: Effective plastic strain to failure. When the plastic strain reaches this value, the element is deleted from the calculation. TDEL Minimum time step size for automatic element deletion. C Strain rate parameter, 𝐶, see formula below. VARIABLE DESCRIPTION P Strain rate parameter, 𝑃, see formula below. LCSS Load curve ID or Table ID. Load Curve. When LCSS is a Load curve ID, it is taken as defining effective stress versus effective plastic strain. If defined EPS1 - EPS8 and ES1 - ES8 are ignored. Tabular Data. The table ID defines for each strain rate value a load curve ID giving the stress versus effective plastic strain for that rate, See Figure M24-1. When the strain rate falls below the minimum value, the stress versus effective plastic strain curve for the lowest value of strain rate is used. Likewise, when the strain rate exceeds the maximum value the stress versus effective plastic strain curve for the highest value of strain rate is used. The strain rate parameters: C and P, the curve ID, LCSR, EPS1 - EPS8, and Linear ES1 - ES8 are ignored if a Table ID is defined. interpolation between the discrete strain rates is used by default; logarithmic the LOG_INTERPOLATION option is invoked. interpolation when used is interpolation between discrete strain rates Logarithmically Defined Tables. An alternative way to invoke logarithmic is described as follows. If the first value in the table is negative, LS- DYNA assumes that all the table values represent the natural logarithm of a strain rate. Since the tables are internally discretized to equally space the table values, it makes good sense from an accuracy standpoint that the table values represent the natural log of strain rate when the lowest strain rate and highest strain rate differ by several orders of magnitude. There is some additional computational cost associated invoking logarithmic interpolation. Load curve ID defining strain rate scaling effect on yield stress. If LCSR is negative, the load curve is evaluated using a binary search for the correct interval for the strain rate. The binary search is slower than the default incremental search, but in cases where large changes in the strain rate may occur over a single time step, it is more robust. This option is not necessary for the viscoplastic formulation. LCSR *MAT_PIECEWISE_LINEAR_PLASTICITY DESCRIPTION VP Formulation for rate effects: EQ.-1.0: Cowper-Symonds with deviatoric strain rate rather than total, EQ.0.0: Scale yield stress (default), EQ.1.0: Viscoplastic formulation. EPS1 - EPS8 Effective plastic strain values (optional; supersedes SIGY, ETAN). At least 2 points should be defined. The first point must be zero corresponding to the initial yield stress. WARNING: If the first point is nonzero the yield stress is extrapolated to determine the initial yield. If this option is used SIGY and ETAN are ignored and may be input as zero. ES1 - ES8 Corresponding yield stress values to EPS1 - EPS8. Remarks: The stress strain behavior may be treated by a bilinear stress strain curve by defining the tangent modulus, ETAN. Alternately, a curve of effective stress vs. effective plastic strain similar to that shown in Figure M10-1 may be defined by (EPS1, ES1) - (EPS8, ES8); however, a curve ID (LCSS) may be referenced instead if eight points are insufficient. The cost is roughly the same for either approach. Note that in the special case of uniaxial stress, true stress vs. true plastic strain is equivalent to effective stress vs. effective plastic strain. The most general approach is to use the table definition (LCSS) discussed below. Three options to account for strain rate effects are possible. 1. Strain rate may be accounted for using the Cowper and Symonds model which scales the yield stress with the factor 1 + ( 𝑝⁄ ) 𝜀̇ where 𝜀̇ is the strain rate. 𝜀̇ = √𝜀̇𝑖𝑗𝜀̇𝑖𝑗. If VP = -1. The deviatoric strain rates are used instead. If the viscoplastic option is active, VP = 1.0, and if SIGY is > 0 then the dynamic 𝑝 ), which is yield stress is computed from the sum of the static stress, 𝜎𝑦 typically given by a load curve ID, and the initial yield stress, SIGY, multiplied by the Cowper-Symonds rate term as follows: 𝑠(𝜀eff 𝜎𝑦(𝜀eff 𝑝 , 𝜀̇eff 𝑝 ) = 𝜎𝑦 𝑠(𝜀eff 𝑝 ) + SIGY × 𝑝⁄ 𝜀̇eff ⎟⎞ 𝐶 ⎠ ⎜⎛ ⎝ where the plastic strain rate is used. With this latter approach similar results can be obtained between this model and material model: *MAT_ANISOTROP- IC_VISCOPLASTIC. If SIGY = 0, the following equation is used instead where 𝑝 ), must be defined by a load curve: the static stress, 𝜎𝑦 𝑠(𝜀eff 𝜎𝑦(𝜀eff 𝑝 , 𝜀̇eff 𝑝 ) = 𝜎𝑦 𝑝 ) 𝑠(𝜀eff 𝜀̇eff ⎟⎞ 𝐶 ⎠ ⎜⎛ ⎝ ⎡ 1 + ⎢⎢ ⎣ 𝑝⁄ ⎤ ⎥⎥ ⎦ This latter equation is always used if the viscoplastic option is off. 2. For complete generality a load curve (LCSR) to scale the yield stress may be input instead. In this curve the scale factor versus strain rate is defined. 3. If different stress versus strain curves can be provided for various strain rates, the option using the reference to a table (LCSS) can be used. Then the table input in *DEFINE_TABLE has to be used, see Figure M24-1. A fully viscoplastic formulation is optional (variable VP) which incorporates the different options above within the yield surface. An additional cost is incurred over the simple scaling but the improvement is results can be dramatic. For implicit calculations on this material involving severe nonlinear hardening the radial return method may result in inaccurate stress-strain response. By setting IACC = 1 on *CONTROL_ACCURACY activates a fully iterative plasticity algorithm, which will remedy this. This is not to be confused with the MITER flag on *CON- TROL_SHELL, which governs the treatment of the plane stress assumption for shell elements. If failure is applied with this option, incident failure will initiate damage, and the stress will continuously degrade to zero before erosion for a deformation of 1% plastic strain. So for instance, if the failure strain is FAIL = 0.05, then the element is eroded when 𝜀̅𝑝 = 0.06 and the material goes from intact to completely damaged between 𝜀̅𝑝 = 0.05 and 𝜀̅𝑝 = 0.06. The reason is to enhance implicit performance by maintaining continuity in the internal forces. For a nonzero failure strain, *DEFINE_MATERIAL_HISTORIES can be used to output the failure indicator. *DEFINE_MATERIAL_HISTORIES Properties Label Attributes Description Instability - - - - Failure indicator 𝜀eff 𝑝 /𝜀fail 𝑝 , see FAIL *DEFINE_MATERIAL_HISTORIES Properties Label Attributes Description Plastic Strain Rate - - - - 𝑝 Effective plastic strain rate 𝜀̇eff *MAT_025 This is Material Type 25. This is an inviscid two invariant geologic cap model. This material model can be used for geomechanical problems or for materials as concrete, see references cited below. Card 1 1 Variable MID 2 RO 3 BULK Type A8 Card 2 Variable Type 1 R F Card 3 1 F 2 D F 2 F 3 W F 3 4 G F 4 X0 F 4 Variable PLOT FTYPE VEC TOFF Type F F F F 5 6 7 8 ALPHA THETA GAMMA BETA F 5 C F 5 F 6 N F 6 F 7 F 8 7 8 VARIABLE MID DESCRIPTION Material identification. A unique number or label not exceeding 8 characters must be specified. RO Mass density. BULK Initial bulk modulus, K. G Initial Shear modulus. ALPHA THETA Failure envelope parameter, α. Failure envelope linear coefficient, θ. GAMMA Failure envelope exponential coefficient, γ. *MAT_GEOLOGIC_CAP_MODEL DESCRIPTION BETA Failure envelope exponent, β. R D W X0 C N Cap, surface axis ratio. Hardening law exponent. Hardening law coefficient. Hardening law exponent, X0. Kinematic hardening coefficient, 𝑐̅. Kinematic hardening parameter. PLOT Save the following variable for plotting in LS-PrePost, to be labeled there as “effective plastic strain:” EQ.1: hardening parameter, κ EQ.2: cap -J1 axis intercept, X(κ) 𝑝 EQ.3: volumetric plastic strain 𝜀𝑣 EQ.4: first stress invariant, 𝐽1 EQ.5: second stress invariant, √𝐽2 EQ.6: not used EQ.7: not used EQ.8: response mode number EQ.9: number of iterations FTYPE Formulation flag: EQ.1: soils (Cap surface may contract) EQ.2: concrete and rock (Cap doesn’t contract) VEC Vectorization flag: EQ.0: vectorized (fixed number of iterations) EQ.1: fully iterative If the vectorized solution is chosen, the stresses might be slightly off the yield surface; however, on vector computers a much more efficient solution is achieved. TOFF Tension Cut Off, TOFF < 0 (positive in compression). J2D J2D = Fe f1 J2D = Fc f2 J1 X(κ) f3 Figure M25-1. The yield surface of the two-invariant cap model in pressure√𝐽2𝐷 − 𝐽1 space. Surface f1 is the failure envelope, f2 is the cap surface, and f3 is the tension cutoff. Remarks: The implementation of an extended two invariant cap model, suggested by Stojko [1990], is based on the formulations of Simo, et al. [1988, 1990] and Sandler and Rubin [1979]. In this model, the two invariant cap theory is extended to include nonlinear kinematic hardening as suggested by Isenberg, Vaughan, and Sandler [1978]. A brief discussion of the extended cap model and its parameters is given below. The cap model is formulated in terms of the invariants of the stress tensor. The square root of the second invariant of the deviatoric stress tensor, √𝐽2𝐷 is found from the deviatoric stresses s as √𝐽2𝐷 ≡ √ 𝑆𝑖𝑗𝑆𝑖𝑗 and is the objective scalar measure of the distortional or shearing stress. The first invariant of the stress, J1, is the trace of the stress tensor. The cap model consists of three surfaces in √𝐽2𝐷 − 𝐽1 space, as shown in Figure M25-1 First, there is a failure envelope surface, denoted f1 in the figure. The functional form of f1 is where Fe is given by 𝑓1 = √𝐽2𝐷 − min[𝐹𝑒(𝐽1), 𝑇mises], 𝐹𝑒(𝐽1) ≡ 𝛼 − 𝛾exp(−𝛽𝐽1) + 𝜃𝐽1 and 𝑇𝑚𝑖𝑠𝑒𝑠 ≡ |𝑋(𝜅𝑛) − 𝐿(𝜅𝑛)|. This failure envelop surface is fixed in √𝐽2𝐷 − 𝐽1 space, and therefore does not harden unless kinematic hardening is present. Next, there is a cap surface, denoted f2 in the figure, with f2 given by 𝑓2 = √𝐽2𝐷 − 𝐹𝑐(𝐽1, 𝐾) where Fc is defined by 𝐹𝑐(𝐽1, 𝜅) ≡ √[𝑋(𝜅) − 𝐿(𝜅)]2 − [𝐽1 − 𝐿(𝜅)]2, 𝑋(𝜅) is the intersection of the cap surface with the J1 axis and 𝐿(𝜅) is defined by 𝑋(𝜅) = 𝜅 + 𝑅𝐹𝑒(𝜅), 𝐿(𝜅) ≡ {𝜅 if 𝜅 > 0 0 if 𝜅 ≤ 0 The hardening parameter κ is related to the plastic volume change 𝜀𝑣 hardening law 𝑝 through the 𝑝 = 𝑊{1 − exp[−𝐷(𝑋(𝜅) − 𝑋0)]} 𝜀𝑣 Geometrically, κ is seen in the figure as the J1 coordinate of the intersection of the cap surface and the failure surface. Finally, there is the tension cutoff surface, denoted f3 in the figure. The function f3 is given by f3 ≡ T − J1 where T is the input material parameter which specifies the maximum hydrostatic tension sustainable by the material. The elastic domain in √𝐽2𝐷 − 𝐽1 space is then bounded by the failure envelope surface above, the tension cutoff surface on the left, and the cap surface on the right. An additive decomposition of the strain into elastic and plastic parts is assumed: 𝜺 = 𝜺𝑒 + 𝜺𝑝, where εe is the elastic strain and εp is the plastic strain. Stress is found from the elastic strain using Hooke’s law, where σ is the stress and C is the elastic constitutive tensor. 𝝈 = 𝑪(𝜺 − 𝜺𝒑), The yield condition may be written 𝑓1(𝑠) ≤ 0 𝑓2(𝑠, 𝜅) ≤ 0 𝑓3(𝑠) ≤ 0 and the plastic consistency condition requires that 𝜆̇𝑘𝑓𝑘 = 0 𝑘 = 1,2,3 𝜆̇𝑘 ≥ 0 where 𝜆𝑘 is the plastic consistency parameter for surface k. If 𝑓𝑘 < 0 then, 𝜆̇𝑘 = 0 and the response is elastic. If 𝑓𝑘 > 0 then surface k is active and 𝜆̇𝑘 is found from the requirement that 𝑓 ̇ 𝑘 = 0. Associated plastic flow is assumed, so using Koiter’s flow rule the plastic strain rate is given as the sum of contribution from all of the active surfaces, 𝜀̇𝑝 = ∑ 𝜆̇𝑘 𝑘=1 ∂𝑓𝑘 ∂𝑠 . One of the major advantages of the cap model over other classical pressure-dependent plasticity models is the ability to control the amount of dilatancy produced under shear loading. Dilatancy is produced under shear loading as a result of the yield surface having a positive slope in √𝐽2𝐷 − 𝐽 space, so the assumption of plastic flow in the direction normal to the yield surface produces a plastic strain rate vector that has a component in the volumetric (hydrostatic) direction . In models such as the Drucker-Prager and Mohr-Coulomb, this dilatancy continues as long as shear loads are applied, and in many cases produces far more dilatancy than is experimental- ly observed in material tests. In the cap model, when the failure surface is active, dilatancy is produced just as with the Drucker-Prager and Mohr-Coulumb models. However, the hardening law permits the cap surface to contract until the cap intersects the failure envelope at the stress point, and the cap remains at that point. The local normal to the yield surface is now vertical, and therefore the normality rule assures that no further plastic volumetric strain (dilatancy) is created. Adjustment of the parameters that control the rate of cap contractions permits experimentally observed amounts of dilatancy to be incorporated into the cap model, thus producing a constitutive law which better represents the physics to be modeled. Another advantage of the cap model over other models such as the Drucker-Prager and Mohr-Coulomb is the ability to model plastic compaction. In these models all purely volumetric response is elastic. In the cap model, volumetric response is elastic until the stress point hits the cap surface. Therefore, plastic volumetric strain (compaction) is generated at a rate controlled by the hardening law. Thus, in addition to controlling the amount of dilatancy, the introduction of the cap surface adds another experimentally observed response characteristic of geological material into the model. The inclusion of kinematic hardening results in hysteretic energy dissipation under cyclic loading conditions. Following the approach of Isenberg, et al. [1978] a nonlinear kinematic hardening law is used for the failure envelope surface when nonzero values of and N are specified. In this case, the failure envelope surface is replaced by a family of yield surfaces bounded by an initial yield surface and a limiting failure envelope surface. Thus, the shape of the yield surfaces described above remains unchanged, but they may translate in a plane orthogonal to the J axis, Translation of the yield surfaces is permitted through the introduction of a “back stress” tensor, α The formulation including kinematic hardening is obtained by replacing the stress σ with the translated stress tensor 𝜂 ≡ 𝜎 − 𝛼 in all of the above equation. The history tensor α is assumed deviatoric, and therefore has only 5 unique components. The evolution of the back stress tensor is governed by the nonlinear hardening law 𝛼 = 𝑐 ̅𝐹̅(𝜎, 𝛼)𝑒 ̇𝑝 where 𝑐 ̅ is a constant, 𝐹̅ is a scalar function of σ and α and 𝑒 ̇𝑝 is the rate of deviatoric plastic strain. The constant may be estimated from the slope of the shear stress - plastic shear strain curve at low levels of shear stress. The function 𝐹̅ is defined as 𝐹̅ ≡ max [0,1 − (𝜎 − 𝛼)𝛼 2𝑁𝐹𝑒(𝐽1) ] where N is a constant defining the size of the yield surface. The value of N may be interpreted as the radial distant between the outside of the initial yield surface and the inside of the limit surface. In order for the limit surface of the kinematic hardening cap model to correspond with the failure envelope surface of the standard cap model, the scalar parameter α must be replaced α - N in the definition Fe. The cap model contains a number of parameters which must be chosen to represent a particular material, and are generally based on experimental data. The parameters α, β, θ, and γ are usually evaluated by fitting a curve through failure data taken from a set of triaxial compression tests. The parameters W, D, and X0 define the cap hardening law. The value W represents the void fraction of the uncompressed sample and D governs the slope of the initial loading curve in hydrostatic compression. The value of R is the ration of major to minor axes of the quarter ellipse defining the cap surface. Additional details and guidelines for fitting the cap model to experimental data are found in Chen and Baladi [1985]. *MAT_026 This is Material Type 26. The major use of this material model is for honeycomb and foam materials with real anisotropic behavior. A nonlinear elastoplastic material behavior can be defined separately for all normal and shear stresses. These are considered to be fully uncoupled. See notes below. Card 1 1 Variable MID 2 RO Type A8 F 3 E F 4 PR F 5 SIGY F 6 VF F 7 8 MU BULK F F Default none none none none none none .05 0.0 Card 2 1 2 3 4 5 6 7 8 Variable LCA LCB LCC LCS LCAB LCBC LCCA LCSR Type F F F F F F F F Default none LCA LCA LCA LCS LCS LCS optional Card 3 1 2 3 4 5 6 7 8 Variable EAAU EBBU ECCU GABU GBCU GCAU AOPT MACF Type F F F F F F Card 4 Variable 1 XP Type F 2 YP F 3 ZP F 4 A1 F 5 A2 F 6 A3 F I 8 Variable 1 D1 Type F *MAT_HONEYCOMB 2 D2 F 3 D3 F 4 5 TSEF SSEF F F 6 V1 F 7 V2 F 8 V3 F VARIABLE DESCRIPTION MID RO E PR Material identification. A unique number or label not exceeding 8 characters must be specified. Mass density. Young’s modulus for compacted honeycomb material. Poisson’s ratio for compacted honeycomb material. SIGY Yield stress for fully compacted honeycomb. VF MU Relative volume at which the honeycomb is fully compacted. μ, material viscosity coefficient. (default=.05) Recommended. BULK Bulk viscosity flag: LCA LCB LCC LCS EQ.0.0: bulk viscosity is not used. This is recommended. EQ.1.0: bulk viscosity is active and μ = 0. This will give results identical to previous versions of LS-DYNA. Load curve ID, see *DEFINE_CURVE, for sigma-aa versus either relative volume or volumetric strain. See notes below. Load curve ID, see *DEFINE_CURVE, for sigma-bb versus either relative volume or volumetric strain. Default LCB = LCA. See notes below. Load curve ID, see *DEFINE_CURVE, for sigma-cc versus either relative volume or volumetric strain. Default LCC = LCA. See notes below. Load curve ID, see *DEFINE_CURVE, for shear stress versus either relative volume or volumetric strain. Default LCS = LCA. Each component of shear stress may have its own load curve. See notes below. VARIABLE LCAB LCBC LCCA LCSR EAAU EBBU ECCU GABU GBCU GCAU AOPT DESCRIPTION Load curve ID, see *DEFINE_CURVE, for sigma-ab versus either relative volume or volumetric strain. Default LCAB = LCS. See notes below. Load curve ID, see *DEFINE_CURVE, for sigma-bc versus either relative volume or volumetric strain. Default LCBC = LCS. See notes below. Load curve ID, see *DEFINE_CURVE, or sigma-ca versus either relative volume or volumetric strain. Default LCCA = LCS. See notes below. Load curve ID, see *DEFINE_CURVE, for strain-rate effects defining the scale factor versus strain rate. This is optional. The curves defined above are scaled using this curve. Elastic modulus Eaau in uncompressed configuration. Elastic modulus Ebbu in uncompressed configuration. Elastic modulus Eccu in uncompressed configuration. Shear modulus Gabu in uncompressed configuration. Shear modulus Gbcu in uncompressed configuration. Shear modulus Gcau in uncompressed configuration. Material axes option : EQ.0.0: locally orthotropic with material axes determined by element nodes 1, 2, and 4, as with *DEFINE_COORDI- NATE_NODES. EQ.1.0: locally orthotropic with material axes determined by a point in space and the global location of the element center; this is the a-direction. EQ.2.0: globally orthotropic with material axes determined by vectors defined below, as with *DEFINE_COORDI- NATE_VECTOR EQ.3.0: locally orthotropic material axes determined by rotating the material axes about the element normal by an angle, BETA, from a line in the plane of the element defined by the cross product of the vector v with the *MAT_HONEYCOMB DESCRIPTION element normal. The plane of a solid element is the midsurface between the inner surface and outer surface defined by the first four nodes and the last four nodes of the connectivity of the element, respectively. EQ.4.0: locally orthotropic in cylindrical coordinate system with the material axes determined by a vector v, and an originating point, p, which define the centerline ax- is. This option is for solid elements only. LT.0.0: the absolute value of AOPT is a coordinate system ID number (CID on *DEFINE_COORDINATE_NODES, *DEFINE_COORDINATE_SYSTEM or *DEFINE_CO- ORDINATE_VECTOR). Available in R3 version of 971 and later.. MACF Material axes change flag: EQ.1: No change, default, EQ.2: switch material axes a and b, EQ.3: switch material axes a and c, EQ.4: switch material axes b and c. XP YP ZP Coordinates of point p for AOPT = 1 and 4. A1 A2 A3 Components of vector a for AOPT = 2. D1 D2 D3 Components of vector d for AOPT = 2. V1 V2 V3 Define components of vector v for AOPT = 3 and 4. Tensile strain at element failure (element will erode). Shear strain at element failure (element will erode). TSEF SSEF Remarks: For efficiency it is strongly recommended that the load curve ID’s: LCA, LCB, LCC, LCS, LCAB, LCBC, and LCCA, contain exactly the same number of points with corresponding strain values on the abscissa. If this recommendation is followed the cost of the table lookup is insignificant. Conversely, the cost increases significantly if the abscissa strain values are not consistent between load curves. The behavior before compaction is orthotropic where the components of the stress tensor are uncoupled, i.e., an a component of strain will generate resistance in the local a-direction with no coupling to the local b and c directions. The elastic moduli vary, from their initial values to the fully compacted values at Vf, linearly with the relative volume V: 𝐸𝑎𝑎 = 𝐸𝑎𝑎𝑢 + 𝛽(𝐸 − 𝐸𝑎𝑎𝑢) 𝐸𝑏𝑏 = 𝐸𝑏𝑏𝑢 + 𝛽(𝐸 − 𝐸𝑏𝑏𝑢) 𝐸𝑐𝑐 = 𝐸𝑐𝑐𝑢 + 𝛽(𝐸 − 𝐸𝑐𝑐𝑢) 𝐺𝑎𝑏 = 𝐸𝑎𝑏𝑢 + 𝛽(𝐺 − 𝐺𝑎𝑏𝑢) 𝐺𝑏𝑐 = 𝐸𝑏𝑐𝑢 + 𝛽(𝐺 − 𝐺𝑏𝑐𝑢) 𝐺𝑐𝑎 = 𝐸𝑐𝑎𝑢 + 𝛽(𝐺 − 𝐺𝑐𝑎𝑢) 𝛽 = max [min ( 1 − 𝑉 1 − 𝑉𝑓 , 1) , 0] where and G is the elastic shear modulus for the fully compacted honeycomb material 𝐺 = 2(1 + 𝑣) . The relative volume, V, is defined as the ratio of the current volume to the initial volume. Typically, V = 1 at the beginning of a calculation. The viscosity coefficient µ (MU) should be set to a small number (usually .02 - .10 is okay). Alternatively, the two bulk viscosity coefficients on the control cards should be set to very small numbers to prevent the development of spurious pressures that may lead to undesirable and confusing results. The latter is not recommended since spurious numerical noise may develop. Curve extends into negative volumetric strain quadrant since LS-DYNA will extrapolate using the two end points. It is important that the extropolation does not extend into the negative σ ij unloading and reloading path Strain: -ε ij Unloading is based on the interpolated Young’s moduli which must provide an unloading tangent that exceeds the loading tangent. Figure M26-1. Stress quantity versus volumetric strain. Note that the “yield stress” at a volumetric strain of zero is non-zero. In the load curve definition, see *DEFINE_CURVE, the “time” value is the volumetric strain and the “function” value is the yield stress. The load curves define the magnitude of the average stress as the material changes density (relative volume), see Figure M26-1. Each curve related to this model must have the same number of points and the same abscissa values. There are two ways to define these curves, a) as a function of relative volume (V) or b) as a function of volumetric strain defined as: 𝜀𝑉 = 1 − 𝑉 In the former, the first value in the curve should correspond to a value of relative volume slightly less than the fully compacted value. In the latter, the first value in the curve should be less than or equal to zero, corresponding to tension, and increase to full compaction. Care should be taken when defining the curves so that extrapolated values do not lead to negative yield stresses. At the beginning of the stress update each element’s stresses and strain rates are transformed into the local element coordinate system. For the uncompacted material, the trial stress components are updated using the elastic interpolated moduli according to: 𝑛+1trial 𝜎𝑎𝑎 𝑛+1trial 𝜎𝑏𝑏 𝑛+1trial 𝜎𝑐𝑐 𝑛+1trial 𝜎𝑎𝑏 = 𝜎𝑎𝑎 = 𝜎𝑏𝑏 = 𝜎𝑐𝑐 = 𝜎𝑎𝑏 𝑛 + 𝐸𝑎𝑎Δ𝜀𝑎𝑎 𝑛 + 𝐸𝑏𝑏Δ𝜀𝑏𝑏 𝑛 + 𝐸𝑐𝑐Δ𝜀𝑐𝑐 𝑛 + 2𝐺𝑎𝑏Δ𝜀𝑎𝑏 𝑛+1trial 𝜎𝑏𝑐 = 𝜎𝑏𝑐 𝑛 + 2𝐺𝑏𝑐Δ𝜀𝑏𝑐 𝑛+1trial 𝜎𝑐𝑎 = 𝜎𝑐𝑎 𝑛 + 2𝐺𝑐𝑎Δ𝜀𝑐𝑎 Each component of the updated stresses is then independently checked to ensure that they do not exceed the permissible values determined from the load curves; e.g., if then 𝑛+1trial ∣𝜎𝑖𝑗 ∣ > 𝜆𝜎𝑖𝑗(𝑉) 𝑛+1 = 𝜎𝑖𝑗(𝑉) 𝜎𝑖𝑗 𝑛+1trial 𝜆𝜎𝑖𝑗 ∣𝜆𝜎𝑖𝑗 𝑛+1trial∣ On Card 2 σij (V) is defined by LCA for the aa stress component, LCB for the bb component, LCC for the cc component, and LCS for the ab, bc, ca shear stress components. The parameter λ is either unity or a value taken from the load curve number, LCSR, that defines λ as a function of strain-rate. Strain-rate is defined here as the Euclidean norm of the deviatoric strain-rate tensor. For fully compacted material it is assumed that the material behavior is elastic-perfectly plastic and the stress components updated according to: where the deviatoric strain increment is defined as trial = 𝑠𝑖𝑗 𝑠𝑖𝑗 𝑑𝑒𝑣 𝑛 + 2𝐺Δ𝜀𝑖𝑗 𝑛+1 2⁄ Δ𝜀𝑖𝑗 dev = Δ𝜀𝑖𝑗 − Δ𝜀𝑘𝑘𝛿𝑖𝑗 Now a check is made to see if the yield stress for the fully compacted material is exceeded by comparing trial = ( 𝑠eff 2⁄ trial) trial𝑠𝑖𝑗 𝑠𝑖𝑗 the effective trial stress to the defined yield stress, SIGY. If the effective trial stress exceeds the yield stress the stress components are simply scaled back to the yield surface Now the pressure is updated using the elastic bulk modulus, K 𝑛+1 = 𝑠𝑖𝑗 𝜎𝑦 trial 𝑠eff trial. 𝑠𝑖𝑗 where 𝑛+1 𝑝𝑛+1 = 𝑝𝑛 − 𝐾Δ𝜀𝑘𝑘 2⁄ 𝐾 = 3(1 − 2𝑣) to obtain the final value for the Cauchy stress 𝑛+1 = 𝑠𝑖𝑗 𝜎𝑖𝑗 𝑛+1 − 𝑝𝑛+1𝛿𝑖𝑗 After completing the stress update transform the stresses back to the global configuration. For *CONSTRAINED_TIED_NODES_WITH_FAILURE, the failure is based on the volume strain instead to the plastic strain. *MAT_MOONEY-RIVLIN_RUBBER This is Material Type 27. A two-parametric material model for rubber can be defined. Card 1 1 Variable MID Type A8 Card 2 1 2 RO F 2 Variable SGL SW Type F F 3 PR F 3 ST F 4 A F 4 LCID F 5 B F 5 6 REF F 6 7 8 7 8 VARIABLE DESCRIPTION MID RO PR A B REF Material identification. A unique number or label not exceeding 8 characters must be specified. Mass density. Poisson’s ratio (value between 0.49 and 0.5 is recommended, smaller values may not work). Constant, see literature and equations defined below. Constant, see literature and equations defined below. Use reference geometry to initialize the stress tensor. The reference geometry is defined by the keyword:*INITIAL_FOAM_- REFERENCE_GEOMETRY . EQ.0.0: off, EQ.1.0: on. If the values on Card 2 are nonzero, then a least squares fit is computed from the uniaxial data provided by the curve LCID superceding the A and B values on Card 1. If the A and B fields are left blank on Card 1 then the variables on Card 2 must be nonzero. SGL Specimen gauge length 𝑙0, see Figure M27-1. *MAT_MOONEY-RIVLIN_RUBBER DESCRIPTION Specimen width, see Figure M27-1. Specimen thickness, see Figure M27-1. Curve ID, see *DEFINE_CURVE, giving the force versus actual change 𝐿 in the gauge length. See also Figure M27-2 for an alternative definition. *MAT_027 VARIABLE SW ST LCID Remarks: The strain energy density function is defined as: 𝑊 = 𝐴(𝐼 − 3) + 𝐵(𝐼𝐼 − 3) + 𝐶(𝐼𝐼𝐼−2 − 1) + 𝐷(𝐼𝐼𝐼 − 1)2 where 𝐶 = 0.5𝐴 + 𝐵 𝐷 = 𝐴(5𝜐 − 2) + 𝐵(11𝜐 − 5) 2(1 − 2𝜐) 𝜈 = Poisson’s ratio 2(𝐴 + 𝐵) = shear modulus of linear elasticity 𝐼, 𝐼𝐼, 𝐼𝐼𝐼 = invariants of right Cauchy-Green Tensor C. The load curve definition that provides the uniaxial data should give the change in gauge length, Δ𝐿, versus the corresponding force. In compression both the force and the change in gauge length must be specified as negative values. In tension the force and change in gauge length should be input as positive values. The principal stretch ratio in the uniaxial direction, 𝜆1, is then given by 𝐿0 + Δ𝐿 𝐿0 𝜆1 = with 𝐿0 being the initial length and 𝐿 being the actual length. Alternatively, the stress versus strain curve can also be input by setting the gauge length, thickness, and width to unity (1.0) and defining the engineering strain in place of the change in gauge length and the nominal (engineering) stress in place of the force, see Figure M27-1. The least square fit to the experimental data is performed during the initialization phase and is a comparison between the fit and the actual input is provided in the d3hsp file. It is a good idea to visually check to make sure it is acceptable. The coefficients 𝐴 and 𝐵 are also printed in the output file. It is also advised to use the material driver for checking out the material model. gauge length Force AA Δ gauge length Section AA thickness width Figure M27-1. Uniaxial specimen for experimental data applied force initial area = A0 change in gauge length gauge length = ∆L Figure M27-2 The stress versus strain curve can used instead of the force versus the change in the gauge length by setting the gauge length, thickness, and width to unity (1.0) and defining the engineering strain in place of the change in gauge length and the nominal (engineering) stress in place of the force. *MAT_077_O is a better alternative for fitting data resembling the curve above. *MAT_027 will provide a poor fit to a curve that exhibits an strong upturn in slope as strains become large. *MAT_RESULTANT_PLASTICITY This is Material Type 28. A resultant formulation for beam and shell elements including elasto-plastic behavior can be defined. This model is available for the Belytschko-Schwer beam, the Co triangular shell, the Belytschko-Tsay shell, and the fully integrated type 16 shell. For beams, the treatment is elastic-perfectly plastic, but for shell elements isotropic hardening is approximately modeled. For a detailed description we refer to the LS-DYNA Theory Manual. Since the stresses are not computed in the resultant formulation, the stresses output to the binary databases for the resultant elements are zero. Card 1 1 Variable MID 2 RO Type A8 F 3 E F 4 PR F 5 6 7 8 SIGY ETAN F F Default none none none none none 0.0 VARIABLE DESCRIPTION MID RO E PR SIGY ETAN Material identification. A unique number or label not exceeding 8 characters must be specified. Mass density Young’s modulus Poisson’s ratio Yield stress Plastic hardening modulus (for shells only) *MAT_029 This is Material Type 29. With this material model, for the Belytschko-Schwer beam only, plastic hinge forming at the ends of a beam can be modeled using curve definitions. Optionally, collapse can also be modeled. See also *MAT_139. Description: FORCE LIMITED Resultant Formulation Card 1 1 Variable MID 2 RO Type A8 F 3 E F 4 PR F 5 DF F 6 7 8 AOPT YTFLAG ASOFT F F F Default none none none none 0.0 0.0 0.0 0.0 Card 2 1 Variable M1 Type F Default none Card 3 1 2 M2 F 0 2 3 M3 F 0 3 4 M4 F 0 4 5 M5 F 0 5 6 M6 F 0 6 7 M7 F 0 7 8 M8 F 0 8 Variable LC1 LC2 LC3 LC4 LC5 LC6 LC7 LC8 Type F Default none F 0 F 0 F 0 F 0 F 0 F 0 F Card 4 1 2 3 4 5 6 7 8 Variable LPS1 SFS1 LPS2 SFS2 YMS1 YMS2 Type Default F 0 F F F F F 1.0 LPS1 1.0 1.0E+20 YMS1 Card 5 1 2 3 4 5 6 7 8 Variable LPT1 SFT1 LPT2 SFT2 YMT1 YMT2 Type Default F 0 F F F F F 1.0 LPT1 1.0 1.0E+20 YMT1 Card 6 1 2 3 4 5 6 7 8 Variable LPR SFR YMR Type Default F 0 F F 1.0 1.0E+20 VARIABLE DESCRIPTION MID RO E PR DF Material identification. A unique number or label not exceeding 8 characters must be specified. Mass density Young’s modulus Poisson’s ratio Damping factor, see definition in notes below. A proper control for the timestep has to be maintained by the user! VARIABLE DESCRIPTION AOPT Axial load curve option: EQ.0.0: axial load curves are force versus strain, EQ.1.0: axial load curves are force versus change in length. LT.0.0: the absolute value of AOPT is a coordinate system ID number (CID on *DEFINE_COORDINATE_NODES, *DEFINE_COORDINATE_SYSTEM or *DEFINE_CO- ORDINATE_VECTOR). Available in R3 version of 971 and later. YTFLAG Flag to allow beam to yield in tension: EQ.0.0: beam does not yield in tension, EQ.1.0: beam can yield in tension. ASOFT M1, M2, …, M8 LC1, LC2, …, LC8 LPS1 SFS1 LPS2 SFS2 YMS1 Axial elastic softening factor applied once hinge has formed. When a hinge has formed the stiffness is reduced by this factor. If zero, this factor is ignored. Applied end moment for force versus (strain/change in length) curve. At least one must be defined. A maximum of 8 moments can be defined. The values should be in ascending order. Load curve ID defining axial force (collapse load) versus strain/change in length for the corresponding applied end moment. Define the same number as end moments. Each curve must contain the same number of points. Load curve ID for plastic moment versus rotation about s-axis at node 1. If zero, this load curve is ignored. Scale factor for plastic moment versus rotation curve about s-axis at node 1. Default = 1.0. Load curve ID for plastic moment versus rotation about s-axis at node 2. Default: is same as at node 1. Scale factor for plastic moment versus rotation curve about s-axis at node 2. Default: is same as at node 1. Yield moment about s-axis at node 1 for interaction calculations (default set to 1.0E+20 to prevent interaction). *MAT_FORCE_LIMITED DESCRIPTION Yield moment about s-axis at node 2 for interaction calculations (default set to YMS1). Load curve ID for plastic moment versus rotation about t-axis at node 1. If zero, this load curve is ignored. Scale factor for plastic moment versus rotation curve about t-axis at node 1. Default = 1.0. Load curve ID for plastic moment versus rotation about t-axis at node 2. Default: is the same as at node 1. Scale factor for plastic moment versus rotation curve about t-axis at node 2. Default: is the same as at node 1. Yield moment about t-axis at node 1 for interaction calculations (default set to 1.0E+20 to prevent interactions) Yield moment about t-axis at node 2 for interaction calculations (default set to YMT1) Load curve ID for plastic torsional moment versus rotation. If zero, this load curve is ignored. Scale factor for plastic torsional moment versus rotation (default = 1.0). Torsional yield moment for interaction calculations (default set to 1.0E+20 to prevent interaction) YMS2 LPT1 SFT1 LPT2 SFT2 YMT1 YMT2 LPR SFR YMR Remarks: This material model is available for the Belytschko resultant beam element only. Plastic hinges form at the ends of the beam when the moment reaches the plastic moment. The moment versus rotation relationship is specified by the user in the form of a load curve and scale factor. The points of the load curve are (plastic rotation in radians, plastic moment). Both quantities should be positive for all points, with the first point being (zero, initial plastic moment). Within this constraint any form of characteristic may be used, including flat or falling curves. Different load curves and scale factors may be specified at each node and about each of the local s and t axes. Axial collapse occurs when the compressive axial load reaches the collapse load. Collapse load versus collapse deflection is specified in the form of a load curve. The points of the load curve are either (true strain, collapse force) or (change in length, collapse force). Both quantities should be entered as positive for all points, and will be interpreted as compressive. The first point should be (zero, initial collapse load). The collapse load may vary with end moment as well as with deflections. In this case several load-deflection curves are defined, each corresponding to a different end moment. Each load curve should have the same number of points and the same deflection values. The end moment is defined as the average of the absolute moments at each end of the beam and is always positive. Stiffness-proportional damping may be added using the damping factor λ. This is defined as follows: 𝜆 = 2 × 𝜉 where ξ is the damping factor at the reference frequency ω (in radians per second). For example if 1% damping at 2Hz is required 𝜆 = 2 × 0.01 2𝜋 × 2 = 0.001592 If damping is used, a small timestep may be required. LS-DYNA does not check this so to avoid instability it may be necessary to control the timestep via a load curve. As a guide, the timestep required for any given element is multiplied by 0.3L⁄cλ when damping is present (L = element length, c = sound speed). Moment Interaction: Plastic hinges can form due to the combined action of moments about the three axes. This facility is activated only when yield moments are defined in the material input. A hinge forms when the following condition is first satisfied. where, ⎜⎛ 𝑀𝑟 ⎟⎞ 𝑀ryield⎠ ⎝ + ⎜⎛ 𝑀𝑠 ⎟⎞ 𝑀syield⎠ ⎝ + ⎜⎛ 𝑀𝑡 ⎟⎞ 𝑀tyield⎠ ⎝ ≥ 1 𝑀𝑟, 𝑀𝑠, 𝑀𝑡, = current moment 𝑀𝑟yield, 𝑀𝑠yield, 𝑀𝑡yield = yield moment Note that scale factors for hinge behavior defined in the input will also be applied to the yield moments: for example, 𝑀𝑠yield in the above formula is given by the input yield moment about the local axis times the input scale factor for the local s axis. For strain- softening characteristics, the yield moment should generally be set equal to the initial peak of the moment-rotation load curve. On forming a hinge, upper limit moments are set. These are given by M8 M7 M6 M5 M4 M3 M2 M1M1 Strain (or change in length, see AOPT) Figure M29-1. The force magnitude is limited by the applied end moment. For an intermediate value of the end moment LS-DYNA interpolates between the curves to determine the allowable force value. 𝑀𝑟upper = max ⎜⎛𝑀𝑟, ⎝ 𝑀𝑟yield ⎟⎞ 2 ⎠ and similar conditions hold for 𝑀𝑠upper and 𝑀𝑡upper. Thereafter, the plastic moments will be given by 𝑀𝑟𝑝 = min(𝑀𝑟upper, 𝑀𝑟curve) where, 𝑀𝑟p = current plastic moment 𝑀𝑟curve = moment from load curve at the current rotation scaled by the scale factor. 𝑀𝑠𝑝and 𝑀𝑡𝑝 satisfy similar conditions. The effect of this is to provide an upper limit to the moment that can be generated; it represents the softening effect of local buckling at a hinge site. Thus if a member is bent about is local s-axis it will then be weaker in torsion and about its local t-axis. For moment-softening curves, the effect is to trim off the initial peak (although if the curves subsequently harden, the final hardening will also be trimmed off). It is not possible to make the plastic moment vary with axial load. *MAT_SHAPE_MEMORY This is material type 30. This material model describes the superelastic response present in shape-memory alloys (SMA), that is the peculiar material ability to undergo large deformations with a full recovery in loading-unloading cycles . The material response is always characterized by a hysteresis loop. See the references by Auricchio, Taylor and Lubliner [1997] and Auricchio and Taylor [1997]. This model is available for shells, solids, and Hughes-Liu beam elements. 5 6 7 8 Card 1 1 Variable MID 2 RO Type A8 F 3 E F 4 PR F Default none none none none Card 2 1 2 3 4 5 6 7 8 Variable SIG_ASS SIG_ASF SIG_SAS SIG_SAF EPSL ALPHA YMRT Type F F F F F F F Default none none none none none 0.0 0.0 Optional Load Curve Card (starting with R7.1). Load curves for mechanically induced phase transitions. Card 3 1 2 3 4 5 6 7 8 Variable LCID_AS LCID_SA Type I I Default none none VARIABLE DESCRIPTION MID RO E PR SIG_ASS SIG_ASF SIG_SAS SIG_SAF EPSL ALPHA YMRT Material identification. A unique number or label not exceeding 8 characters must be specified. Density Young’s modulus Poisson’s ratio Starting value for the forward phase transformation (conversion of austenite into martensite) in the case of a uniaxial tensile state of stress. A load curve for SIG_ASS as a function of temperature is specified by using the negative of the load curve ID number. Final value for the forward phase transformation (conversion of austenite into martensite) in the case of a uniaxial tensile state of stress. SIG_ASF as a function of temperature is specified by using the negative of the load curve ID number. Starting value for the reverse phase transformation (conversion of martensite into austenite) in the case of a uniaxial tensile state of stress. SIG_SAS as a function of temperature is specified by using the negative of the load curve ID number. Final value for the reverse phase transformation (conversion of martensite into austenite) in the case of a uniaxial tensile state of stress. SIG_SAF as a function of temperature is specified by using the negative of the load curve ID number. Recoverable strain or maximum residual strain. It is a measure of the maximum deformation obtainable all the martensite in one direction. Parameter measuring the difference between material responses in tension and compression (set alpha = 0 for no difference). Also, see the following Remark. Young’s modulus for the martensite if it is different from the modulus for the austenite. Defaults to the austenite modulus if it is set to zero. LCID_AS Load curve ID or Table ID for the forward phase change (conversion of austenite into martensite). 1. When LCID_AS is a load curve ID the curve is taken to be *MAT_SHAPE_MEMORY DESCRIPTION effective stress versus martensite fraction (ranging from 0 to 1). 2. When LCID_AS is a table ID the table defines for each phase transition rate (derivative of martensite fraction) a load curve ID specifying the stress versus martensite fraction for that phase transition rate. The stress versus martensite fraction curve for the lowest value of the phase transition rate is used, if the phase transition rate falls below the minimum value. Likewise, the stress versus martensite fraction curve for the highest value of phase transition rate is used if phase transition rate exceeds the maximum value. 3. The values of SIG_ASS and SIG_ASF are overwritten when this option is used. LCID_SA Load curve ID or Table ID for reverse phase change (conversion of martensite into austenite). 1. When LCID_SA is a load curve ID the curve is taken to be effective stress versus martensite fraction (ranging from 0 to 1). 2. When LCID_SA is a table ID the table defines for each phase transition rate (derivative of martensite fraction) a load curve ID specifying the stress versus martensite fraction for that phase transition rate. The stress versus martensite fraction curve for the lowest value of the phase transition rate is used, if the phase transition rate falls below the minimum value. Likewise, the stress versus martensite fraction curve for the highest value of phase transition rate is used if phase transition rate exceeds the maximum value. 3. The values of SIG_ASS and SIG_ASF are overwritten when this option is used. Remarks: The material parameter alpha, α, measures the difference between material responses in tension and compression. In particular, it is possible to relate the parameter α to the σAX σAS σSA σSA (cid:3) (cid:3)L Figure M30-1. Superelastic Behavior for a Shape Memory Material initial stress value of the austenite into martensite conversion, indicated respectively as 𝐴𝑆,+ and 𝜎𝑠 𝜎𝑠 𝐴𝑆,−, according to the following expression: 𝛼 = 𝐴𝑆,− − 𝜎𝑠 𝜎𝑠 𝐴𝑆,− + 𝜎𝑠 𝜎𝑠 𝐴𝑆,+ 𝐴𝑆,+ In the following, the results obtained from a simple test problem is reported. The material properties are set as: E PR 60000 MPa 0.3 SIG_ASS 520 MPa SIG_ASF 600 MPa SIG_SAS 300 MPa SIG_SAF 200 MPa 1000 500 -500 -1000 -0.1 -0.05 0.05 True Strain Figure M30-2. Complete loading-unloading test in tension and compression. EPSL 0.07 ALPHA 0.12 YMRT 50000 MPa The investigated problem is the complete loading-unloading test in tension and compression. The uniaxial Cauchy stress versus the logarithmic strain is plotted in Figure M30-2. *MAT_FRAZER_NASH_RUBBER_MODEL This is Material Type 31. This model defines rubber from uniaxial test data. It is a modified form of the hyperelastic constitutive law first described in Kenchington [1988]. See also the notes below. Card 1 1 Variable MID Type A8 Card 2 1 2 RO F 2 3 PR F 3 4 5 6 7 8 C100 C200 C300 C400 F 4 F 5 F 6 F 7 8 Variable C110 C210 C010 C020 EXIT EMAX EMIN REF Type F Card 3 1 F 2 Variable SGL SW Type F F F 3 ST F F 4 LCID F F 5 F 6 F 7 F 8 VARIABLE DESCRIPTION MID RO PR C100 C200 C300 Material identification. A unique number or label not exceeding 8 characters must be specified. Mass density. Poisson’s ratio. Values between .49 and .50 are suggested. C100 (EQ.1.0 if term is in the least squares fit.) C200 (EQ.1.0 if term is in the least squares fit.) C300 (EQ.1.0 if term is in the least squares fit.) C400 C110 C210 C010 C020 EXIT *MAT_FRAZER_NASH_RUBBER_MODEL DESCRIPTION C400 (EQ.1.0 if term is in the least squares fit.) C110 (EQ.1.0 if term is in the least squares fit.) C210 (EQ.1.0 if term is in the least squares fit.) C010 (EQ.1.0 if term is in the least squares fit.) C020 (EQ.1.0 if term is in the least squares fit.) Exit option: EQ.0.0: stop if strain limits are exceeded (recommended), NE.0.0: continue if strain limits are exceeded. The curve is then extrapolated. EMAX Maximum strain limit, (Green-St, Venant Strain). EMIN Minimum strain limit, (Green-St, Venant Strain). Use reference geometry to initialize the stress tensor. The reference geometry is defined by the keyword: *INITIAL_- FOAM_REFERENCE_GEOMETRY . EQ.0.0: off, EQ.1.0: on. Specimen gauge length, see Figure M27-1. Specimen width, see Figure M27-1. Specimen thickness, see Figure M27-1. Load curve ID, see DEFINE_CURVE, giving the force versus actual change in gauge length. See also Figure M27-2 for an alternative definition. REF SGL SW ST LCID Remarks: The constants can be defined directly or a least squares fit can be performed if the uniaxial data (SGL, SW, ST and LCID) is available. If a least squares fit is chosen, then the terms to be included in the energy functional are flagged by setting their corresponding coefficients to unity. If all coefficients are zero the default is to use only the terms involving I1 and I2. C100 defaults to unity if the least square fit is used. The strain energy functional, U, is defined in terms of the input constants as: 𝑈 = 𝐶100𝐼1 + 𝐶200𝐼1 2 + 𝐶300𝐼1 3 + 𝐶400𝐼1 4 + 𝐶110𝐼1𝐼2 + 𝐶210𝐼1 2𝐼2 + 𝐶010𝐼2 + 𝐶020𝐼2 2 + 𝑓 (𝐽) where the invariants can be expressed in terms of the deformation gradient matrix, Fij, and the Green-St. Venant strain tensor, Eij : 𝐽 = ∣𝐹𝑖𝑗∣ 𝐼1 = 𝐸𝑖𝑖 𝐼2 = 2! 𝑖𝑗 𝐸𝑝𝑖𝐸𝑞𝑗 𝛿𝑝𝑞 The derivative of U with respect to a component of strain gives the corresponding component of stress here, Sij, is the second Piola-Kirchhoff stress tensor. 𝑆𝑖𝑗 = ∂𝑈 ∂𝐸𝑖𝑗 The load curve definition that provides the uniaxial data should give the change in gauge length, ΔL, and the corresponding force. In compression both the force and the change in gauge length must be specified as negative values. In tension the force and change in gauge length should be input as positive values. The principal stretch ratio in the uniaxial direction, λ1, is then given by 𝜆 = 𝐿𝑜 + Δ𝐿 𝐿𝑜 Alternatively, the stress versus strain curve can also be input by setting the gauge length, thickness, and width to unity and defining the engineering strain in place of the change in gauge length and the nominal (engineering) stress in place of the force, see Figure M27-2 The least square fit to the experimental data is performed during the initialization phase and is a comparison between the fit and the actual input is provided in the printed file. It is a good idea to visually check the fit to make sure it is acceptable. The coefficients C100 - C020 are also printed in the output file. *MAT_LAMINATED_GLASS This is Material Type 32. With this material model, a layered glass including polymeric layers can be modeled. Failure of the glass part is possible. See notes below. Card 1 1 Variable MID Type A8 Card 2 1 2 RO F 2 3 EG F 3 Variable PRP SYP ETP Type F F F 4 5 6 7 PRG SYG ETG EFG F 4 F 5 F 6 F 7 8 EP F 8 Integration Point Cards. Define 1-4 cards specifying up to 32 values. If less than 4 cards are input, reading is stopped by a “*” control card. Card 3 Variable 1 F1 Type F 2 F2 F 3 F3 F 4 F4 F 5 F5 F 6 F6 F 7 F7 F 8 F8 F VARIABLE DESCRIPTION MID RO EG PRG SYG ETG Material identification. A unique number or label not exceeding 8 characters must be specified. Mass density Young’s modulus for glass Poisson’s ratio for glass Yield stress for glass Plastic hardening modulus for glass DESCRIPTION *MAT_032 EFG EP PRP SYP ETP Plastic strain at failure for glass Young’s modulus for polymer Poisson’s ratio for polymer Yield stress for polymer Plastic hardening modulus for polymer F1, …, FN Integration point material: fn = 0.0: glass, fn = 1.0: polymer. A user-defined integration rule must be specified, see *INTEGRA- TION_SHELL. See remarks below. Remarks: Isotropic hardening for both materials is assumed. The material to which the glass is bonded is assumed to stretch plastically without failure. A user defined integration rule specifies the thickness of the layers making up the glass. Fi defines whether the integration point is glass (0.0) or polymer (1.0). The material definition, Fi, has to be given for the same number of integration points (NIPTS) as specified in the rule. A maximum of 32 layers is allowed. If the recommended user defined rule is not defined, the default integration rules are used. The location of the integration points in the default rules are defined in the *SEC- TION_SHELL keyword description. *MAT_BARLAT_ANISOTROPIC_PLASTICITY This is Material Type 33. This model was developed by Barlat, Lege, and Brem [1991] for modeling anisotropic material behavior in forming processes. The finite element implementation of this model is described in detail by Chung and Shah [1992] and is used here. It is based on a six parameter model, which is ideally suited for 3D continuum problems, see notes below. For sheet forming problems, material 36 based on a 3-parameter model is recommended. Card 1 1 Variable MID Type A8 Card 2 Variable Type 1 A F Card 3 1 2 RO F 2 B F 2 Variable AOPT BETA Type F F Card 4 Variable 1 XP Type F 2 YP F 3 E F 3 C F 3 3 ZP F 4 PR F 4 F F 4 4 A1 F 5 K F 5 G F 5 5 A2 F 6 E0 F 6 H F 6 6 A3 F 7 N F 7 LCID F 7 8 M F 8 8 7 Card 5 Variable 1 V1 Type F 2 V2 F 3 V3 F 4 D1 F 5 D2 F 6 D3 F 7 8 VARIABLE MID DESCRIPTION Material identification. A unique number or label not exceeding 8 characters must be specified. RO E PR K EO N M A B C F G H LCID Mass density. Young’s modulus, 𝐸. Poisson’s ratio, 𝜈. 𝑘, strength coefficient, see notes below. 𝜀0, strain corresponding to the initial yield, see notes below. 𝑛, hardening exponent for yield strength. 𝑚, flow potential exponent in Barlat’s Model. 𝑎, anisotropy coefficient in Barlat’s Model. 𝑏, anisotropy coefficient in Barlat’s Model. 𝑐, anisotropy coefficient in Barlat’s Model. 𝑓 , anisotropy coefficient in Barlat’s Model. 𝑔, anisotropy coefficient in Barlat’s Model. ℎ, anisotropy coefficient in Barlat’s Model. Option load curve ID defining effective stress versus effective plastic strain. If nonzero, this curve will be used to define the yield stress. The load curve is implemented for solid elements only. *MAT_BARLAT_ANISOTROPIC_PLASTICITY DESCRIPTION AOPT Material axes option: EQ.0.0: locally orthotropic with material axes determined by element nodes 1, 2, and 4, as with *DEFINE_COORDI- NATE_NODES, and then, for shells only, rotated about the shell element normal by an angle BETA.. EQ.1.0: locally orthotropic with material axes determined by a point in space and the global location of the element center, this is the 𝑎-direction. EQ.2.0: globally orthotropic with material axes determined by vectors defined below, as with *DEFINE_COORDI- NATE_VECTOR. EQ.3.0: locally orthotropic material axes determined by offsetting the material axes by an angle, BETA, from a line determined by taking the cross product of the vec- tor 𝐯 with the normal to the plane of the element. LT.0.0: the absolute value of AOPT is a coordinate system ID number (CID on *DEFINE_COORDINATE_NODES, *DEFINE_COORDINATE_SYSTEM or *DEFINE_CO- ORDINATE_VECTOR). BETA Material angle in degrees for AOPT = 1 (shells only) and AOPT = 3, may be overridden on the element card, see *ELE- MENT_SHELL_BETA or *ELEMENT_SOLID_ORTHO. MACF Material axes change flag for brick elements: EQ.1: No change, default, EQ.2: switch material axes 𝑎 and 𝑏, EQ.3: switch material axes 𝑎 and 𝑐, EQ.4: switch material axes 𝑏 and 𝑐. XP, YP, ZP Coordinates of point 𝐩 for AOPT = 1. A1, A2, A3 Components of vector 𝐚 for AOPT = 2. V1, V2, V3 Components of vector 𝐯 for AOPT = 3. D1, D2, D3 Components of vector 𝐝 for AOPT = 2. Remarks: The yield function Φ is defined as: Φ = |𝑆1 − 𝑆2|𝑚 + ∣𝑆2 − 𝑆3∣𝑚 + ∣𝑆3 − 𝑆1∣𝑚 = 2𝜎̅̅̅̅̅ 𝑚 where 𝜎̅̅̅̅̅ is the effective stress and 𝑆𝑖=1,2,3 are the principal values of the symmetric matrix 𝑆𝛼𝛽, 𝑆𝑥𝑥 = [𝑐(𝜎𝑥𝑥 − 𝜎𝑦𝑦) − 𝑏(𝜎𝑧𝑧 − 𝜎𝑥𝑥)] 3⁄ 𝑆𝑦𝑦 = [𝑎(𝜎𝑦𝑦 − 𝜎𝑧𝑧) − 𝑐(𝜎𝑥𝑥 − 𝜎𝑦𝑦)] 3⁄ 𝑆𝑧𝑧 = [𝑏(𝜎𝑧𝑧 − 𝜎𝑥𝑥) − 𝑎(𝜎𝑦𝑦 − 𝜎𝑧𝑧)] 3⁄ 𝑆𝑦𝑧 = 𝑓 𝜎𝑦𝑧 𝑆𝑧𝑥 = 𝑔𝜎𝑧𝑥 𝑆𝑥𝑦 = ℎ𝜎𝑥𝑦 The material constants a, b, c, f, g and h represent anisotropic properties. When 𝑎 = 𝑏 = 𝑐 = 𝑓 = 𝑔 = ℎ = 1, the material is isotropic and the yield surface reduces to the Tresca yield surface for 𝑚 = 1 and von Mises yield surface for 𝑚 = 2 or 4. For face centered cubic (FCC) materials 𝑚 = 8 is recommended and for body centered cubic (BCC) materials 𝑚 = 6 is used. The yield strength of the material is 𝜎𝑦 = 𝑘(𝜀𝑝 + 𝜀0)𝑛 where 𝜀0 is the strain corresponding to the initial yield stress and 𝜀𝑝 is the plastic strain. *MAT_BARLAT_YLD96 This is Material Type 33. This model was developed by Barlat, Maeda, Chung, Yanagawa, Brem, Hayashida, Lege, Matsui, Murtha, Hattori, Becker, and Makosey [1997] for modeling anisotropic material behavior in forming processes in particular for aluminum alloys. This model is available for shell elements only. Card 1 1 Variable MID Type A8 Card 2 Variable 1 E0 Type F Card 3 Variable 1 C1 Type F Card 4 1 2 RO F 2 N F 2 C2 F 2 3 E F 3 ESR0 F 3 C3 F 3 4 PR F 4 M F 4 C4 F 4 5 K F 5 HARD F 5 AX F 5 6 7 8 6 A F 6 AY F 6 7 8 7 8 AZ0 AZ1 F 7 F 8 Variable AOPT BETA Type F 1 2 3 Variable Type Card 6 Variable 1 V1 Type F 2 V2 F 3 V3 F *MAT_033_96 7 8 7 8 6 A3 F 6 D3 F 4 A1 F 4 D1 F 5 A2 F 5 D2 F DESCRIPTION VARIABLE MID RO E PR K EO N ESR0 M Material identification. A unique number or label not exceeding 8 characters must be specified. Mass density. Young’s modulus, 𝐸. Poisson’s ratio,𝜈. 𝑘, strength coefficient or a in Voce, see notes below. 𝜀0, strain corresponding to the initial yield or b in Voce, see notes below. 𝑛, hardening exponent for yield strength or c in Voce. 𝜀SR0, in powerlaw rate sensitivity. 𝑚, exponent for strain rate effects HARD Hardening option: LT.0.0: absolute value defines the load curve ID. EQ.1.0: powerlaw EQ.2.0: Voce A C1 Flow potential exponent. 𝑐1, see equations below. VARIABLE DESCRIPTION C2 C3 C4 AX AY AZ0 AZ1 𝑐2, see equations below. 𝑐3, see equations below. 𝑐4, see equations below. 𝑎𝑥, see equations below. 𝑎𝑦, see equations below. 𝑎𝑧0, see equations below. 𝑎𝑧1, see equations below. AOPT Material axes option: EQ.0.0: locally orthotropic with material axes determined by element nodes 1, 2, and 4, as with *DEFINE_COORDI- NATE_NODES, and then rotated about the shell ele- ment normal by an angle BETA. EQ.2.0: globally orthotropic with material axes determined by vectors defined below, as with *DEFINE_COORDI- NATE_VECTOR. EQ.3.0: locally orthotropic material axes determined by offsetting the material axes by an angle, BETA, from a line determined by taking the cross product of the vec- tor 𝐯 with the normal to the plane of the element. LT.0.0: the absolute value of AOPT is a coordinate system ID number (CID on *DEFINE_COORDINATE_NODES, *DEFINE_COORDINATE_SYSTEM or *DEFINE_CO- ORDINATE_VECTOR). BETA Material angle in degrees for AOPT = 0 and 3, may be overridden on the element card, see *ELEMENT_SHELL_BETA.. A1, A2, A3 Components of vector 𝐚 for AOPT = 2. V1, V2, V3 Components of vector 𝐯 for AOPT = 3. D1, D2, D3 Components of vector 𝐝 for AOPT = 2. *MAT_033_96 The yield stress 𝜎𝑦 is defined three ways. The first, the Swift equation, is given in terms of the input constants as: 𝜎𝑦 = 𝑘(𝜀0 + 𝜀𝑝)𝑛 ( 𝜀̇ 𝜀𝑆𝑅0 ) The second, the Voce equation, is defined as: 𝜎𝑦 = 𝑎 − 𝑏𝑒−𝑐𝜀𝑝 and the third option is to give a load curve ID that defines the yield stress as a function of effective plastic strain. The yield function Φ is defined as: Φ = 𝛼1|𝑠1 − 𝑠2|𝑎 + 𝛼2∣𝑠2 − 𝑠3∣𝑎 + 𝛼3∣𝑠3 − 𝑠1∣𝑎 = 2𝜎𝑦 𝑎 where 𝑠𝑖 is a principle component of the deviatoric stress tensor where in vector notation: and 𝐋 is given as 𝐬 = 𝐋𝛔 𝐋 = 𝑐2 + 𝑐3 −𝑐3 −𝑐2 ⎡ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎣ −𝑐3 𝑐3 + 𝑐1 −𝑐1 3 −𝑐2 −𝑐1 𝑐1 + 𝑐2 ⎤ ⎥ ⎥ ⎥ ⎥ ⎥ ⎥ ⎥ 𝑐4⎦ A coordinate transformation relates the material frame to the principle directions of 𝐬 is used to obtain the 𝛼𝑘 coefficients consistent with the rotated principle axes: 2 + 𝛼𝑦𝑝2𝑘 2 2 + 𝛼𝑧𝑝3𝑘 𝛼𝑘 = 𝛼𝑥𝑝1𝑘 𝛼𝑧 = 𝛼𝑧0cos2(2𝛽) + 𝛼𝑧1sin2(2𝛽) where 𝑝𝑖𝑗 are components of the transformation matrix. The angle 𝛽 defines a measure of the rotation between the frame of the principal value of 𝐬 and the principal anisotropy axes. *MAT_FABRIC This is Material Type 34. This material is especially developed for airbag materials. The fabric model is a variation on the layered orthotropic composite model of material 22 and is valid for 3 and 4 node membrane elements only. In addition to being a constitutive model, this model also invokes a special membrane element formulation which is more suited to the deformation experienced by fabrics under large deformation. For thin fabrics, buckling can result in an inability to support compressive stresses; thus a flag is included for this option. A linearly elastic liner is also included which can be used to reduce the tendency for these elements to be crushed when the no-compression option is invoked. In LS-DYNA versions after 931 the isotropic elastic option is available. 2 RO F 2 3 EA F 3 Card 1 1 Variable MID Type A8 Card 2 1 Variable GAB Type F Remarks Card 3 1 2 3 4 EB F 4 CSE F 1 4 5 6 7 8 PRBA PRAB F 6 F 7 8 PRL LRATIO DAMP F 4 6 F 4 7 F 8 5 EL F 4 5 Variable AOPT FLC/X2 FAC/X3 ELA LNRC FORM FVOPT TSRFAC Type F Remarks F 2 F 2 F 3 F 4 F 11 F 9 F 10 BETA ISREFG F I 8 7 RL F *MAT_FABRIC *MAT_034 Card 4 1 2 3 Variable RGBRTH A0REF Type F F Card 5 Variable 1 V1 Type F 2 V2 F 3 V3 F 4 A1 F 4 5 A2 F 5 6 A3 F 6 7 X0 F 7 8 X1 F 8 Additional card for FORM = 4, 14, or -14. Card 6 1 2 3 4 5 6 Variable LCA LCB LCAB LCUA LCUB LCUAB Type I I I I I I Additional card for FORM = -14. Card 7 1 2 Variable LCAA LCBB Type I I 3 H F 4 DT F 5 6 7 8 ECOAT SCOAT TCOAT F F F VARIABLE MID DESCRIPTION Material identification. A unique number or label not exceeding 8 characters must be specified. RO Mass density. VARIABLE DESCRIPTION EA EB PRBA PRAB GAB Young’s modulus - longitudinal direction. For an isotopic elastic fabric material only EA and PRBA are defined and are used as the isotropic Young’s modulus and Poisson’s ratio, respectively. The input for the fiber directions and liner should be input as zero for the isotropic elastic fabric Young’s modulus - transverse direction, set to zero for isotropic elastic material. 𝜈𝑏𝑎, Minor Poisson’s ratio ba direction. 𝜈𝑎𝑏, Major Poisson’s ratio ab direction. 𝐺𝑎𝑏, shear modulus ab direction, set to zero for isotropic elastic material. CSE Compressive stress elimination option : EL PRL LRATIO DAMP AOPT EQ.0.0: don’t eliminate compressive stresses, (default) EQ.1.0: eliminate compressive stresses. This option does not apply to the liner. Young’s modulus for elastic liner (required if LRATIO > 0). Poisson’s ratio for elastic liner (required if LRATIO > 0). A non-zero value activates the elastic liner and defines the ratio of liner thickness to total fabric thickness (optional). Rayleigh damping coefficient. A 0.05 coefficient is recommended corresponding to 5% of critical damping. Sometimes larger values are necessary. Material axes option . Also, please refer to Remark 5 for additional information specific to fibre directions for fabrics: EQ.0.0: locally orthotropic with material axes determined by element nodes 1, 2, and 4, as with *DEFINE_COORDI- NATE_NODES, and then rotated about the element normal by an angle BETA. EQ.2.0: globally orthotropic with material axes determined by vectors defined below, as with *DEFINE_COORDI- NATE_VECTOR. *MAT_034 DESCRIPTION EQ.3.0: locally orthotropic material axes determined by rotating the material axes about the element normal by an angle, BETA, from a line in the plane of the element defined by the cross product of the vector v with the element nor- mal. LT.0.0: the absolute value of AOPT is a coordinate system ID number (CID on *DEFINE_COORDINATE_NODES, *DEFINE_COORDINATE_SYSTEM or *DEFINE_CO- ORDINATE_VECTOR). Available in R3 version of 971 and later. If X0 is between 0 and 1 (exclusive) then X2 (FLC) X3 (FAC) X2 is a coefficient of the porosity from the equation in Anagonye and Wang [1999]. X3 is a coefficient of the porosity equation of Anagonye and Wang [1999]. Else If X0 = 0 or -1 then (sets meaning of the abscissa for load curve cases) FLC (X2) Optional porous leakage flow coefficient. GE.0: Porous leakage flow coefficient. LT.0: |FLC| is interpreted as a load curve ID defining FLC as a function of time. If FVOPT < 7 then (sets meaning of the mantissa for load curve case) FAC (X3) Optional characteristic fabric parameter. GE.0: Characteristic fabric parameter LT.0: |FAC| is interpreted as a load curve ID defining FAC as a function of absolute pressure. VARIABLE DESCRIPTION Else if FVOPT ≥ 7 then (sets meaning of the mantissa for load curve case) FAC (X3) Optional characteristic fabric parameter. GE.0: Characteristic fabric parameter LT.0: |FAC| is interpreted as a load curve ID giving leakage volume flux rate versus absolute pressure. The volume flux (per area) rate (per time) has the unit of 𝑑(volflux) dt⁄ ≈ [length]3 ([length]2[time]) , ≈ [length] [time] ⁄ ⁄ equivalent to relative porous gas speed. End if Else if X0 = 1 (sets meaning of the abscissa for load curve cases) FLC (X2) Optional porous leakage flow coefficient. GE.0: Porous leakage flow coefficient. LT.0: |FLC| is interpreted as a load curve curve ID defining FLC versus the stretching ratio defined as 𝑟𝑠 = 𝐴/𝐴0. See notes below. If FVOPT > 7 then (sets meaning of the mantissa for load curve case) FAC (X3) Optional characteristic fabric parameter. GE.0: Characteristic fabric parameter LT.0: |FAC| is interpreted as a load curve defining FAC versus the pressure ratio 𝑟𝑝 = 𝑃ai𝑟/𝑃bag. See Remark 2 below. DESCRIPTION *MAT_034 Else if FVOPT ≥ 7 then (sets meaning of the mantissa for load curve case) FAC (X3) Optional characteristic fabric parameter. GE.0: Characteristic fabric parameter LT.0: |FAC| is interpreted as a load curve defining leakage volume flux rate versus the pressure ratio defined as 𝑟𝑝 = 𝑃air/𝑃bag. See Remark 2 below. The volume flux (per area) rate (per time) has the unit of 𝑑(volflux) dt⁄ ≈ [length]3 ([length]2[time]) , ≈ [length] [time] ⁄ ⁄ equivalent to relative porous gas speed. End if End if ELA Effective leakage area for blocked fabric, ELA : LT.0.0: |ELA| is the load curve ID of the curve defining ELA versus time. The default value of zero assumes that no leakage occurs. A value of .10 would assume that 10% of the blocked fabric is leaking gas. LNRC Flag to turn off compression in liner until the reference geometry is reached, i.e., the fabric element becomes tensile. EQ.0.0: off. EQ.1.0: on. FORM Flag to modify membrane formulation for fabric material: EQ.0.0: default. Least costly and very reliable. EQ.1.0: invariant local membrane coordinate system EQ.2.0: Green-Lagrange strain formulation EQ.3.0: EQ.4.0: large strain with nonorthogonal material angles. See Remark 5. large strain with nonorthogonal material angles and nonlinear stress strain behavior. Define optional load curve IDs on optional card. EQ.12.0: Enhanced version of formulation 2. See Remark 11. VARIABLE DESCRIPTION EQ.13.0: Enhanced version of formulation 3. See Remark 11. EQ.14.0: Enhanced version of formulation 4. See Remark 11. EQ.-14.0: Same as formulation 14, but invokes reading of card 7. See Remark 14. EQ.24.0: Enhanced version of formulation 14. See Remark 11. FVOPT Fabric venting option. EQ.1: Wang-Nefske formulas for venting through an orifice are used. Blockage is not considered. EQ.2: Wang-Nefske formulas for venting through an orifice are used. Blockage of venting area due to contact is consid- ered. EQ.3: Leakage formulas of Graefe, Krummheuer, and Siejak [1990] are used. Blockage is not considered. EQ.4: Leakage formulas of Graefe, Krummheuer, and Siejak [1990] are used. Blockage of venting area due to contact is considered. EQ.5: Leakage formulas based on flow through a porous media are used. Blockage is not considered. EQ.6: Leakage formulas based on flow through a porous media are used. Blockage of venting area due to contact is con- sidered. EQ.7: Leakage is based on gas volume outflow versus pressure load curve [Lian, 2000]. Blockage is not considered. Abso- lute pressure is used in the porous-velocity-versus- pressure load curve, given as FAC in the *MAT_FABRIC card. EQ.8: Leakage is based on gas volume outflow versus pressure load curve [Lian 2000]. Blockage of venting or porous area due to contact is considered. Absolute pressure is used in the porous-velocity-versus-pressure load curve, given as FAC in the *MAT_FABRIC card. DESCRIPTION TSRFAC Strain restoration factor *MAT_034 LT.0: |TSRFAC| is the ID of a curve defining TSRFAC versus time.. GT.0 and LT.1: TSRFAC applied from time 0. GE.1: TSRFAC is the ID of a curve that defines TSRFAC versus time using an alternate method (not available for FORM = 0 or 1). RGBRTH Material dependent birth time of airbag reference geometry. Non- zero RGBRTH overwrites the birth time defined in the *AIRBAG_- REFERENCE_GEOMETRY_BIRTH section. RGBRTH also applies to reference geometry defined by *AIRBAG_SHELL_REFER- ENCE_GEOMETRY. A0REF Calculation option of initial area, A0, used for airbag porosity leakage calculation. EQ.0.: default. Use the initial geometry defined in *NODE. EQ.1.: Use the reference geometry *AIRBAG_REFERENCE_GEOMETRY *AIRBAG_SHELL_REFERENCE_GEOMETRY. defined in or A1, A2, A3 Components of vector a for AOPT = 2. X0, X1 Coefficients of Anagonye and Wang [1999] porosity equation for the leakage area: 𝐴leak = 𝐴0(𝑋0 + 𝑋1𝑟𝑠 + 𝑋2𝑟𝑝 + 𝑋3𝑟𝑠𝑟𝑝) X0.EQ.-1: Compressing seal vent option. The leakage area is evaluated as 𝐴leak = max(𝐴current − 𝐴0, 0). V1, V2, V3 Components of vector 𝐯 for AOPT = 3. BETA ISREFG Material angle in degrees for AOPT = 0 and 3, may be overridden on the element card, see *ELEMENT_SHELL_BETA. Initialize stress by *AIRBAG_REFERENCE_GEOMETRY. This option applies only to FORM = 12. Note that *MAT_FABRIC cannot be initialized using a dynain file because *INITIAL_- STRESS_SHELL is not applicable to *MAT_FABRIC. EQ.0.0: default. Not active. EQ.1.0: active LCA LCB LCAB LCUA LCUB LCUAB RL LCAA *MAT_FABRIC DESCRIPTION Load curve or table ID. Load curve ID defines the stress versus uniaxial strain along the a-axis fiber. Table ID defines for each strain rate a load curve representing stress versus uniaxial strain along the a-axis fiber. Available for FORM = 4, 14, –14, and 24 only, table allowed only for form = -14. If zero, EA is used. For FORM = 14, -14, and 24, this curve can be defined in both tension and compression, see Remark 6 below. Load curve or table ID. Load curve ID defines the stress versus uniaxial strain along the b-axis fiber. Table ID defines for each strain rate a load curve representing stress versus uniaxial strain along the b-axis fiber. Available for FORM = 4, 14, -14, and 24 only, table allowed only for form = -14. If zero, EB is used. For FORM = 14, -14, and 24, this curve can be defined in both tension and compression, see Remark 6 below. Load curve ID for shear stress versus shear strain in the ab-plane; available for FORM = 4, 14, -14, and 24 only. If zero, GAB is used. Unload/reload curve ID for stress versus strain along the a-axis fiber; available for FORM = 4, 14, -14, and 24 only. If zero, LCA is used. Unload/reload curve ID for stress versus strain along the b-axis fiber; available for FORM = 4, 14, -14, and 24 only. If zero, LCB is used. Unload/reload curve ID for shear stress versus shear strain in the ab-plane; available for FORM = 4, 14, -14, and 24 only. If zero, LCAB is used. Optional reloading parameter for FORM = 14 and 24. Values between 0.0 (reloading on unloading curve-default) and 1.0 (reloading on a minimum linear slope between unloading curve and loading curve) are possible. Load curve or table ID. Load curve ID defines the stress along the a-axis fiber versus biaxial strain. Table ID defines for each directional strain rate a load curve representing stress along the a- axis fiber versus biaxial strain. Available for FORM=–14 only, if zero, LCA is used. LCBB *MAT_034 DESCRIPTION Load curve or table ID. Load curve ID defines the stress along the b-axis fiber versus biaxial strain. Table ID defines for each directional strain rate a load curve representing stress along the b- axis fiber versus biaxial strain. Available for FORM=–14 only, if zero, LCB is used. H DT Normalized hysteresis parameter between 0 and 1. Strain rate averaging option. EQ.0.0: Strain rate is evaluated using a running average. LT.0.0: Strain rate is evaluated using average of last 11 time steps. GT.0.0: Strain rate is averaged over the last DT time units. ECOAT Young’s modulus of coat material, see Remark 14. SCOAT Yield stress of coat material, see Remark 14. TCOAT Thickness of coat material, may be positive or negative, see Remark 14. Remarks: 1. The Compressive Stress Elimination Option for Airbag Wrinkling. Setting CSE=1 switches off compressive stress in the fabric, thereby eliminating wrin- kles. Without this “no compression” option the geometry of the bag’s wrinkles control the amount of mesh refinement. In eliminating the wrinkles, this fea- ture reduces the number of elements needed to attain an accurate solution. The no compression option can allow elements to collapse to a line which can lead to elements becoming tangled. The elastic liner option is one way to add some stiffness in compression to prevent this, see Remark 4. Alternatively, when using fabric formulations 14, -14, or 24 tangling can be re- duced by defining stress/strain curves that include negative strain and stress values. See Remark 6.use 2. Porosity. The parameters FLC and FAC are optional for the Wang-Nefske and Hybrid inflation models. It is possible for the airbag to be constructed of multi- ple fabrics having different values for porosity and permeability. Typically, FLC and FAC must be determined experimentally and their variations in time or with pressure are optional to allow for maximum flexibility. 3. Effects of Airbag-Structure Interaction on Porosity. To calculate the leakage of gas through the fabric it is necessary to accurately determine the leakage area. The dynamics of the airbag may cause the leakage area to change during the course of the simulation. In particular, the deformation may change the leakage area, but the leakage area may also decrease when the contact between the airbag and the structure blocks the flow. LS-DYNA can check the interac- tion of the bag with the structure and split the areas into regions that are blocked and unblocked depending on whether the regions are in or not in con- tact, respectively. Blockage effects may be controlled with the ELA field. 4. Elastic Liner. An optional elastic liner can be defined using EL, PRL and LRATIO. The liner is an isotropic layer that acts in both tension and compres- sion. However, setting, LNRC to 1.0 eliminates compressive stress in the liner until both principle stresses are tensile. The compressive stress elimination option, CSE=1, has no influence on the liner behavior. 5. Fiber Axes. For formulations 0, 1, and 2, the 𝑎-axis and 𝑏-axis fiber directions are assumed to be orthogonal and are completely defined by the materi- al axes option, AOPT=0, 2, or 3. For FORM=3, 4, 13, or 14, the fiber directions are not assumed orthogonal and must be specified using the ICOMP=1 option on *SECTION_SHELL. Offset angles should be input into the B1 and B2 fields used normally for integration points 1 and 2. The 𝑎-axis and 𝑏-axis directions will then be offset from the 𝑎-axis direction as determined by the material axis option, AOPT=0, 2, or 3. 6. Stress vs. Strain Curves. For formulations 4, 14, -14, and 24, 2nd Piola-Kirchhoff stress vs. Green’s strain curves may be defined for 𝑎-axis, 𝑏- axis, and shear stresses for loading and also for unloading and reloading. Al- ternatively, the 𝑎-axis and 𝑏-axis curves can be input using engineering stress vs. strain by setting DATYP = -2 on *DEFINE_CURVE. Additionally, for formulations 14, -14, and 24, the uniaxial loading curves LCA and LCB may be defined for negative values of strain and stress, i.e., a straight- forward extension of the curves into the compressive region. This is available in order to model the compressive stresses resulting from tight folding of air- bags. The 𝑎-axis and 𝑏-axis stress follow the curves for the entire defined strain region and if compressive behavior is desired the user should preferably make sure the curve covers all strains of interest. For strains below the first point on the curve, the curve is extrapolated using the stiffness from the constant values, EA or EB. Shear stress/strain behavior is assumed symmetric and curves should be de- fined for positive strain only. However, formulations 14, -14, and 24 allow the extending of the curves in the negative strain region to model asymmetric be- havior. The asymmetric option cannot be used with a shear stress unload curve. If a load curve is omitted, the stress is calculated from the appropriate constant modulus, EA, EB, or GAB. 7. Yield Behavior. When formulations 4, 14, -14, and 24 are used with loading and unloading curves the initial yield strain is set equal to the strain of the first point in the load curve having a stress greater than zero. When the current strain exceeds the yield strain, the stress follows the load curve and the yield strain is updated to the current strain. When unloading occurs, the unload/reload curve is shifted along the x-axis until it intersects the load curve at the current yield strain. When using unloading curves, compres- sive stress elimination should be active to prevent the fibers from developing compressive stress during unloading when the strain remains tensile. To use this option, the unload curve should have a nonnegative second derivate so that the curve will shift right as the yield stress increases. If LCUA, LCUB, or LCUAB are input with negative values, then unloading is handled differently. Instead of shifting the unload curve along the 𝑥-axis, the curve is stretched in both the 𝑥-direction and 𝑦-direction such that the first point remains anchored at (0,0) and the initial intersection point of the curves is moved to the current yield point. This option guarantees the stress remains tensile while the strain is tensile so compressive stress elimination is not neces- sary. To use this option the unload curve should have an initial slope less steep than the load curve, and should steepen such that it intersects the load curve at some positive strain value. 8. Shear Unload-Reload, Fabric Formulation, and LS-DYNA version. With release 6.0.0 of version 971, LS-DYNA changed the way that unload/reload curves for shear stress-strain relations are interpreted. Let f be the shear stress unload-reload curve LCUAB. Then, where the scale factors 𝑐1 and 𝑐2 depend on the fabric form and version of LS-DYNA. 𝜎𝑎𝑏 = 𝑐2𝑓 (𝑐1𝜀𝑎𝑏) Fabric form 4 14 and -14 24 LS971 R5.1.0 and earlier LS971 R6.0.0 to R7.0 LS-DYNA R7.1 and later 𝑐1 2 2 2 𝑐2 1 1 1 𝑐1 2 1 1 𝑐2 1 2 2 𝑐1 𝑐2 - - 1 - - 1 When switching fabric forms or versions, the curve scale factors SFA and SFO on *DEFINE_CURVE can be used to offset this behavior. 9. Per Material Venting Option. The FVOPT flag allows an airbag fabric venting equation to be assigned to a material. The anticipated use for this option is to allow a vent to be defined using FVOPT=1 or 2 for one material and fabric leak- age to be defined for using FVOPT=3, 4, 5, or 6 for other materials. In order to use FVOPT, a venting option must first be defined for the airbag using the OPT parameter on *AIRBAG_WANG_NEFSKE or *AIRBAG_HYBRID. If OPT=0, then FVOPT is ignored. If OPT is defined and FVOPT is omitted, then FVOPT is set equal to OPT. 10. TSRFAC option to restore element strains. Airbags that use a reference geometry will typically have nonzero strains at the start of the calculation. To prevent such initial strains from prematurely opening an airbag, initial strains are stored and subtracted from the measured strain throughout the calculation. 𝝈 = 𝑓 (𝜺 − 𝜺initial) • Fabric formulations 2, 3, and 4 subtract off only the initial ten- sile strains so these forms are typically used with CSE = 1 and LNRC = 1. • Fabric formulations 12, 13, 14, -14, and 24 subtract off the total initial strains so these forms may be used with CSE = 0 or 1 and LNRC = 0 or 1. A side effect of this strain modification is that airbags may not achieve the correct volume when they open. Therefore, the TSRFAC option is imple- mented to reduce the stored initial strain values over time thereby restor- ing the total stain which drives the airbag towards the correct volume. During each cycle, the stored initial strains are scaled by (1.0 − TSRFAC). A small value on the order of 0.0001 is typically sufficient to restore the strains in a few milliseconds of simulation time. The adjustment to restore initial strain is then, 𝝈 = 𝑓 (𝜺 − 𝜺adjustment) 𝛆adjustment = εinitial ∏[1 − TSFRAC] . a) Time Dependent TSRFAC. When TSRFAC ˂ 0, |TSRFAC| becomes the ID of a curve that defines TSRFAC as a function of time. To delay the effect of TSRFAC, the curve ordinate value should be initially zero and should ramp up to a small number to restore the strain at an appropriate time during the simulation. The adjustment to restore initial strain is then, 𝛆adjustment(𝑡𝑖) = εinitial ∏[1 − TSFRAC(𝑡𝑖)] . To prevent airbags from opening prematurely, it is recommended to use the load curve option of TSRFAC to delay the strain restoration until the airbag is partially opened due to pressure loading. b) Alternate Time Dependent TSRFAC. For fabric formulations 2 and higher, a second curve option is invoked by setting TSRFAC≥1 where TSRFAC is again the ID of a curve that defines TSRFAC versus time. Like the first curve option, the stored initial strain values are scaled by (1.0 − TSRFAC), but the modified initial strains are not saved, so the effect of TSRFAC does not accumulate. In this case the adjustment to eliminate initial strain 𝛆adjustment(𝑡𝑖) = [1 − TSFRAC(𝑡𝑖)]𝛆initial. Therefore, the curve should ramp up from zero to one to fully restore the strain. This option gives the user better control of the rate of restoring the strain as it is a function of time rather than solution time step. 11. Enhancements to the Material Formulations. Material formulations 12, 13, and 14 are enhanced versions of formulations 2, 3, and 4, respec- tively. The most notable difference in their behavior is apparent when a refer- ence geometry is used for the fabric. As discussed in Remark 10, the strain is modified to prevent initial strains from prematurely opening an airbag at the start of a calculation. Formulations 2, 3, and 4 subtract the initial tensile strains, while the enhanced formulations subtract the total initial strains. Therefore, the enhanced formula- tions can be used without setting CSE = 1 and LNRC = 1 since compressive stress cutoff is not needed to prevent initial airbag movement. Formulations 2, 3, and 4 need compressive stress cutoff when used with a reference geometry or they can generate compressive stress at the start of a calculation. Available for formulation 12 only, the ISREFG parameter activates an option to calculate the initial stress by using a reference geometry. Material formulation 24 is an enhanced version of formulation 14 implementing a correction for Poisson’s effects when stress vs. strain curves are input for the 𝑎-fiber or 𝑏-fiber. Also, for formulation 24, the outputted stress and strain in the S A2 A1 loading unloading reloading E Figure M34-1. elout or d3plot database files is engineering stress and strain rather than the 2nd Piola Kirchoff and Green’s strain used by formulations other than 0 and 1. 12. Noise Reduction for the Strain Rate Measure. If tables are used, then the strain rate measure is the time derivative of the Green-Lagrange strain in the direction of interest. To suppress noise, the strain rate is averaged according to the value of DT. If DT > 0, it is recommended to use a large enough value to suppress the noise, while being small enough to not lose important information in the signal. 13. Hysteresis. The hysteresis parameter H defines the fraction of dissipated energy during a load cycle in terms of the maximum possible dissipated ener- gy. Referring to the Figure M34-1, 𝐻 ≈ 𝐴1 𝐴1 + 𝐴2 14. Coating Feature for Additional Rotational Resistance. It is possible to model coating of the fabric using a sheet of elastic-ideal-plastic material where the Young’s modulus, yield stress and thickness is specified for the coat materi- al. This will add rotational resistance to the fabric for a more realistic behavior of coated fabrics. To read this parameters set FORM=-14, which adds an extra card containing the three parameters ECOAT, SCOAT and TCOAT, corre- sponding to the three coat material properties mentioned above. The thickness, TCOAT, applies to both sides of the fabric. The coat material for a certain fabric element deforms along with this and all elements connected to this element, which is how the rotations are "captured". Note that unless TCOAT is set to a negative value, the coating will add to the membrane stiff- ness. For negative values of TCOAT the thickness is set to |TCOAT| and the membrane contribution from the coating is suppressed. For this feature to work, the fabric parts must not include any T-intersections, and all of the sur- face normal vectors of connected fabric elements must point in the same direc- tion. This option increases the computational complexity of this material. 15 Fabric forms 12, 13, 14, -14, and 24 allow input of both the minor Poisson’s ratio, 𝜈𝑏𝑎, and the major Poisson’s ratio, 𝜈𝑎𝑏. This allows asymmetric Poisson’s behavior to be modelled. If the major Poisson’s ratio is left blank or input as zero, then it will be calculated using 𝜈𝑎𝑏 = 𝜈𝑏𝑎 . 𝐸𝑎 𝐸𝑏 *MAT_FABRIC_MAP This is Material Type 34 in which the stress response is given exclusively by tables, or maps, and where some obsolete features in *MAT_FABRIC have been deliberately excluded to allow for a clean input and better overview of the model. Card 1 1 Variable MID 2 RO 3 4 5 6 PXX PYY SXY DAMP Type A8 F F Card 2 1 Variable FVOPT Type F Card 3 1 2 X0 F 2 3 X1 F 3 F 4 F 5 F 6 FLC/X2 FAC/X3 ELA F 4 F 5 F 6 7 TH F 7 7 Variable ISREFG CSE SRFAC BULKC JACC FXX FYY Type F Card 4 1 F 2 F 3 F 4 Variable AOPT ECOAT SCOAT TCOAT Type F F F F Card 5 Variable 1 XP Type F 2 YP F 3 ZP F 4 A1 F F 5 5 A2 F F 6 6 A3 F F 7 7 8 2-246 (EOS) LS-DYNA R10.0 8 8 8 DT Variable 1 V1 Type F 2 V2 F 3 V3 F 4 D1 F 5 D2 F 6 D3 F VARIABLE DESCRIPTION *MAT_034M 7 8 BETA F MID RO PXX PYY SXY Material identification. A unique number or label not exceeding 8 characters must be specified. Mass density. Table giving engineering local 𝑋𝑋-stress as function of engineering local 𝑋𝑋-strain and 𝑌𝑌-strain. Table giving engineering local 𝑌𝑌-stress as function of engineering local 𝑌𝑌-strain and 𝑋𝑋-strain. Curve giving local 2nd Piola-Kirchhoff XY-stress as function of local Green 𝑋𝑌-strain. DAMP Damping coefficient for numerical stability. TH Table giving hysteresis factor 0 ≤ 𝐻 < 1 as function of engineering local 𝑋𝑋-strain and 𝑌𝑌-strain. GT.0.0: TH is table ID LE.0.0: -TH is used as constant value for hysteresis factor FVOPT Fabric venting option, see *MAT_FABRIC. X0, X1 Fabric venting option parameters, see *MAT_FABRIC. FLC/X2 Fabric venting option parameter, see *MAT_FABRIC. FAC/X3 Fabric venting option parameter, see *MAT_FABRIC. ELA Fabric venting option parameter, see *MAT_FABRIC. ISREFG Initial stress by reference geometry. EQ.0.0: Not active. EQ.1.0: Active VARIABLE DESCRIPTION CSE Compressive stress elimination option. EQ.0.0: Don’t eliminate compressive stresses, EQ.1.0: Eliminate compressive stresses. SRFAC Load curve ID for smooth stress initialization when using a reference geometry. BULKC Bulk modulus for fabric compaction. JACC FXX FYY Jacobian for the onset of fabric compaction. Load curve giving scale factor of uniaxial stress in first material direction as function of engineering strain rate. Load curve giving scale factor of uniaxial stress in second material direction as function of engineering strain rate. DT Time window for smoothing strain rates used for FXX and FYY. AOPT Material axes option, see *MAT_FABRIC. ECOAT Young’s modulus of coat material to include bending properties. This together with the following two parameters (SCOAT and TCOAT) encompass the same coating/bending feature as in *MAT_FABRIC. Please refer to these manual pages and associated remarks. SCOAT Yield stress of coat material, see *MAT_FABRIC. TCOAT Thickness of coat material, may be positive or negative, see *MAT_FABRIC. A1, A2, A3 Components of vector 𝐚 for AOPT = 2. V1, V2, V3 Components of vector 𝐯 for AOPT = 3. D1, D2, D3 Components of vector 𝐝 for AOPT = 2. BETA Material angle in degrees for AOPT = 0 and 3, may be overridden on the element card, see *ELEMENT_SHELL_BETA. *MAT_034M This material model invokes a special membrane element formulation regardless of the element choice. It is an anisotropic hyperelastic model where the 2nd Piola-Kirchhoff stress 𝐒 is a function of the Green-Lagrange strain 𝐄 and possibly its history. Due to anisotropy, this strain is transformed to obtain the strains in each of the fiber directions 𝐸𝑋𝑋 and 𝐸𝑌𝑌 together with the shear strain 𝐸𝑋𝑌. The associated stress components in the local system are given as functions of the strain components 𝑆𝑋𝑋 = γ𝑆𝑋𝑋(𝐸𝑋𝑋, 𝐸𝑌𝑌)ϑ 𝑆𝑌𝑌 = γ𝑆𝑌𝑌(𝐸𝑌𝑌, 𝐸𝑋𝑋)ϑ 𝑆𝑋𝑌 = γ𝑆𝑋𝑌(𝐸𝑋𝑌)ϑ. The factor 𝛾 is used for dissipative effects and is described in more detail later, for TH = 0, 𝛾 = 1, and the function ϑ represents a strain rate scale factor also described below, for FXX = FYY = 0 this factor is 1. While the shear relation is given directly through the curve SXY, the tabular input of the fiber stress components PXX and PYY is for the sake of convenience the engineering stress as function of engineering strain, i.e., 𝑃𝑋𝑋 = 𝑃𝑋𝑋(𝑒𝑋𝑋, 𝑒𝑌𝑌) 𝑃𝑌𝑌 = 𝑃𝑌𝑌(𝑒𝑌𝑌, 𝑒𝑋𝑋). To this end, the following conversion formulae are used between stresses and strains 𝑒 = √1 + 2𝐸 − 1 𝑆 = 1 + 𝑒 these being applied in each of the two fiber directions. Compressive stress elimination is optional through the CSE parameter, and when activated the principal components of the 2nd Piola-Kirchhoff stress is restricted to positive values. If a reference geometry is used, then SRFAC is the identity of a curve that is a function 𝛼(𝑡) that should increase from zero to unity during a short time span, during which the Green-Lagrange strain used in the formulae above is substituted for 𝐄̃ = 𝐄 − [1 − 𝛼(𝑡)]𝐄0, where 𝑬0 is the strain at time zero. This is done in order to smoothly initialize the stress resulting from using a reference geometry different from the geometry at time zero. The factor 𝛾 is a function of the strain history and is initially set to unity, and depends, more specifically, on the internal work 𝜖 given by the stress power 𝜖 ̇ = 𝐒 ∶ 𝐄̇. Figure M34M-1. Cyclic loading model for hysteresis model H The evolution of 𝛾 is related to the stress power in the sense that it will increase on loading and decrease on unloading, and in this way introduce dissipation. The exact mathematical formula is too complicated to reveal, but in essence the function looks like 𝛾 = { 1 − 𝐻(𝑒 ̅𝑋𝑋, 𝑒𝑌𝑌) + 𝐻(𝑒 ̅𝑋𝑋, 𝑒𝑌𝑌)exp[𝛽(𝜖 − 𝜖)] 1 − 𝐻(𝑒 ̅𝑋𝑋, 𝑒𝑌𝑌)exp[−𝛽(𝜖 − 𝜖)] 𝜖 ̇ < 0 𝜖 ̇ ≥ 0 Here 𝜖 is the maximum attained internal work up to this point in time, 𝑒 ̅𝑋𝑋 and 𝑒 ̅𝑌𝑌 are the engineering strain values associated with value. 𝐻(𝑒 ̅𝑋𝑋, 𝑒𝑌𝑌) is the hysteresis factor defined by the user through the input parameter TH, it may or may not depend on the strains. 𝛽 is a decay constant that depends on 𝑒 ̅𝑋𝑋 and 𝑒 ̅𝑌𝑌, and 𝜖 is the minimum attained internal work at any point in time after 𝜖 was attained. In other words, on unloading 𝛾 will exponentially decay to 1 − 𝐻 and on loading it will exponentially grow to 1 and always be restricted by the lower and upper bounds, 1 − 𝐻 < 𝛾 ≤ 1. The only thing the user needs to care about is to input a proper hysteresis factor 𝐻, and with reference to a general loading/unloading cycle illustrated in figure M34M-1 below the relation 1 − 𝐻 = 𝜖𝑢/𝜖𝑙 should hold. To account for the packing of yarns in compression, a compaction effect is modeled by adding a term to the strain energy function on the form 𝑊𝑐 = 𝐾𝑐𝐽 {𝑙𝑛 ( 𝐽𝑐 ) − 1} , for 𝐽 ≤ 𝐽𝑐 where 𝐾𝑐 (BULKC) is a physical bulk modulus, 𝐽 = det(𝑭) is the jacobian of the deformation and 𝐽𝑐 (JACC) is the critical jacobian for when the effect commences. Here 𝐅 is the deformation gradient. This gives a contribution to the pressure given by 𝑝 = 𝐾𝑐𝑙𝑛 ( 𝐽𝑐 ) , for 𝐽 ≤ 𝐽𝑐 and thus prevents membrane elements from collapsing or inverting when subjected to compressive loads. The bulk modulus 𝐾𝑐 should be selected with the slopes in the stress map tables in mind, presumably some order of magnitude(s) smaller. As an option, the local membrane stress can be scaled based on the engineering strain rates via the function 𝜗 = 𝜗(𝑒 ̇, 𝐒). We set 𝑒 ̇ = max ( 𝜖 ̇ ‖𝐅𝐒‖ , 0) to be the equivalent engineering strain rate in the direction of loading and define 𝜗(𝑒 ̇, 𝑺) = 𝐹𝑋𝑋(𝑒 ̇)|𝑆𝑋𝑋| + 𝐹𝑌𝑌(𝑒 ̇)|𝑆𝑌𝑌| + 2|𝑆𝑋𝑌| |𝑆𝑋𝑋| + |𝑆𝑌𝑌| + 2|𝑆𝑋𝑌| , meaning that the strain rate scale factor defaults to the user input data FXX and FYY for uniaxial loading in the two material directions, respectively. Note that we only consider strain rate scaling in loading and not in unloading, and furthermore that the strain rates used in evaluating the curves are pre-filtered using the time window DT to avoid excessive numerical noise. To this end, it is recommended to set DT to a time corresponding to at least hundred time steps or so. *MAT_PLASTIC_GREEN-NAGHDI_RATE This is Material Type 35. This model is available only for brick elements and is similar to model 3, but uses the Green-Naghdi Rate formulation rather than the Jaumann rate for the stress update. For some cases this might be helpful. This model also has a strain rate dependency following the Cowper-Symonds model. Card 1 1 Variable MID Type A8 Card 2 1 2 RO F 2 3 E F 3 4 PR F 4 5 6 7 8 5 6 7 8 Variable SIGY ETAN SRC SRP BETA Type F F F F F VARIABLE DESCRIPTION MID RO E PR SIGY ETAN SRC SRP BETA Material identification. A unique number or label not exceeding 8 characters must be specified. Density Young’s modulus Poisson’s ratio Yield stress Plastic hardening modulus Strain rate parameter, C Strain rate parameter, P Hardening parameter, 0 < β′ < 1 *MAT_3-PARAMETER_BARLAT_{OPTION} This is Material Type 36. This model was developed by Barlat and Lian [1989] for modeling sheets with anisotropic materials under plane stress conditions. This material allows the use of the Lankford parameters for the definition of the anisotropy. This particular development is due to Barlat and Lian [1989]. A version of this material model which has a flow limit diagram failure option is *MAT_FLD_3-PARAME- TER_BARLAT. Available options include: <BLANK> NLP The NLP option estimates failure using the Formability Index (F.I.), which accounts for the non-linear strain paths seen in metal forming applications . The NLP field in card 3 must be defined when using this option. The NLP option is also available in *MAT_037, *MAT_125 and *MAT_226. Card 1 1 Variable MID Type A8 Card 2 Variable Type 1 M F 2 RO F 2 3 E F 3 4 PR F 4 5 HR F 5 R00/AB R45/CB R90/HB LCID F F F I 6 P1 F 6 E0 F 7 P2 F 7 SPI F 8 ITER F 8 P3 F Define the following card if and only if M < 0 Card opt. 1 2 3 4 5 6 7 8 Variable CRC1 CRA1 CRC2 CRA2 CRC3 CRA3 CRC4 CRA4 Type F F F F F F F 1 Variable AOPT Type F Card 4 1 Variable Type Card 5 Variable 1 V1 Type F Optional card. 2 C F 2 2 V2 F 3 P F 3 3 V3 F *MAT_3-PARAMETER_BARLAT 4 5 6 7 8 VLCID PB NLP/HTA HTB F I/F I 4 A1 F 4 D1 F F 8 7 HTC HTD F 7 F 8 BETA HTFLAG F F 5 A2 F 5 D2 F 6 A3 F 6 D3 F Card 6 1 2 3 4 5 6 7 8 Variable USRFAIL LCBI LCSH Type F F F VARIABLE DESCRIPTION MID RO E Material identification. A unique number or label not exceeding 8 characters must be specified. Mass density. Young’s modulus, 𝐸 GT.0.0: Constant value, LT.0.0: Load curve ID = (-E) which defines Young’s Modulus as a function of plastic strain. See Remarks. VARIABLE DESCRIPTION PR HR Poisson’s ratio, ν Hardening rule: EQ.1.0: linear (default), EQ.2.0: exponential (Swift) EQ.3.0: load curve or table with strain rate effects EQ.4.0: exponential (Voce) EQ.5.0: exponential (Gosh) EQ.6.0: exponential (Hocket-Sherby) EQ.7.0: load curves in three directions EQ.8.0: table with temperature dependence EQ.9.0: 3d table with temperature and strain rate dependence P1 Material parameter: HR.EQ.1.0: Tangent modulus, HR.EQ.2.0: 𝑘, strength coefficient for Swift exponential hard- ening HR.EQ.4.0: 𝑎, coefficient for Voce exponential hardening HR.EQ.5.0: 𝑘, strength coefficient for Gosh exponential hard- ening HR.EQ.6.0: 𝑎, coefficient for Hocket-Sherby exponential hard- ening HR.EQ.7.0: load curve ID for hardening in 45 degree direction. See Remarks. P2 Material parameter: HR.EQ.1.0: Yield stress HR.EQ.2.0: 𝑛, exponent for Swift exponential hardening HR.EQ.4.0: 𝑐, coefficient for Voce exponential hardening HR.EQ.5.0: 𝑛, exponent for Gosh exponential hardening HR.EQ.6.0: 𝑐, coefficient for Hocket-Sherby exponential hard- ening HR.EQ.7.0: load curve ID for hardening in 90 degree direction. See Remarks. *MAT_3-PARAMETER_BARLAT DESCRIPTION ITER Iteration flag for speed: ITER.EQ.0.0: fully iterative ITER.EQ.1.0: fixed at three iterations M CRCn CRAn R00 Generally, ITER = 0 is recommended. However, ITER = 1 is somewhat faster and may give acceptable results in most problems. 𝑚, exponent in Barlat’s yield surface, absolute value is used if negative. Chaboche-Rousselier hardening parameters, see Remarks. Chaboche-Rousselier hardening parameters, see Remarks. 𝑅00, Lankford parameter in 0 degree direction GT.0.0: Constant value, LT.0.0: Load curve or Table ID = (-R00) which defines 𝑅 value as a function of plastic strain (Curve) or as a function of temperature and plastic strain (Table). See Remarks. R45 𝑅45, Lankford parameter in 45 degree direction GT.0.0: Constant value, LT.0.0: Load curve or Table ID = (-R45) which defines R value as a function of plastic strain (Curve) or as a function of temperature and plastic strain (Table). See Remarks. R90 𝑅90, Lankford parameter in 90 degree direction GT.0.0: Constant value, LT.0.0: Load curve or Table ID = (-R90) which defines R value as a function of plastic strain (Curve) or as a function of temperature and plastic strain (Table). See Remarks. AB CB HB LCID 𝑎, Barlat89 parameter, which is read instead of R00 if PB > 0. 𝑐, Barlat89 parameter, which is read instead of R45 if PB > 0. ℎ, Barlat89 parameter, which is read instead of R90 if PB > 0. Load curve/table ID for hardening in the 0 degree direction. See Remarks. VARIABLE DESCRIPTION E0 Material parameter HR.EQ.2.0: 𝜀0 for determining initial yield stress for Swift exponential hardening. (Default = 0.0) HR.EQ.4.0: 𝑏, coefficient for Voce exponential hardening HR.EQ.5.0: 𝜀0 for determining initial yield stress for Gosh exponential hardening. (Default = 0.0) HR.EQ.6.0: 𝑏, coefficient for Hocket-Sherby exponential hard- ening SPI Case I: if 𝜀0 is zero above and HR.EQ.2.0. (Default = 0.0) [1 ⁄ ] (𝑛−1) EQ.0.0: 𝜀0 = (𝐸 𝑘) LE.0.02: 𝜀0 = SPI GT.0.02: 𝜀0 = (SPI 𝑘 ) [1 𝑛⁄ ] Case II: If HR.EQ.5.0 The strain at plastic yield is determined by an iterative procedure based on the same principles as for HR.EQ.2.0. P3 Material parameter: HR.EQ.5.0: 𝑝, parameter for Gosh exponential hardening HR.EQ.6.0: 𝑛, exponent for Hocket-Sherby exponential hardening AOPT Material axes option : EQ.0.0: locally orthotropic with material axes determined by element nodes 1, 2, and 4, as with *DEFINE_COORDI- NATE_NODES, and then rotated about the shell ele- ment normal by an angle BETA. EQ.2.0: globally orthotropic with material axes determined by vectors defined below, as with *DEFINE_COORDI- NATE_VECTOR. EQ.3.0: locally orthotropic material axes determined by rotating the material axes about the element normal by an angle, BETA, from a line in the plane of the element defined by the cross product of the vector v with the element normal. C P VLCID PB NLP HTA HTB *MAT_3-PARAMETER_BARLAT DESCRIPTION LT.0.0: the absolute value of AOPT is a coordinate system ID number (CID on *DEFINE_COORDINATE_NODES, *DEFINE_COORDINATE_SYSTEM or *DEFINE_CO- ORDINATE_VECTOR). Available with the R3 release of Version 971 and later. 𝐶 in Cowper-Symonds strain rate model 𝑝 in Cowper-Symonds strain rate model, 𝑝 = 0.0 for no strain rate effects Volume correction curve ID defining the relative volume change (change in volume relative to the initial volume) as a function of the effective plastic strain. This is only used when nonzero. See Remarks. Barlat89 parameter, p. If PB > 0, parameters AB, CB, and HB are read instead of R00, R45, and R90. See Remarks below. ID of a load curve of the Forming Limit Diagram (FLD) under linear strain paths. In the load curve, abscissas represent minor strains while ordinates represent major strains. Define only when option NLP is used. See Remarks. Load curve/Table ID for postforming parameter A in heat treatment Load curve/Table ID for postforming parameter B in heat treatment XP, YP, ZP Coordinates of point 𝐩 for AOPT = 1. A1, A2, A3 Components of vector 𝐚 for AOPT = 2. HTC HTD Load curve/Table ID for postforming parameter C in heat treatment Load curve/Table ID for postforming parameter D in heat treatment V1, V2, V3 Components of vector 𝐯 for AOPT = 3. D1, D2, D3 Components of vector 𝐝 for AOPT = 2. VARIABLE BETA DESCRIPTION Material angle in degrees for AOPT = 0 and 3, may be overridden on the element card, see *ELEMENT_SHELL_BETA. HTFLAG Heat treatment flag : HTFLAG.EQ.0: Preforming stage HTFLAG.EQ.1: Heat treatment stage HTFLAG.EQ.2: Postforming stage USRFAIL User defined failure flag USRFAIL.EQ.0: no user subroutine is called USRFAIL.EQ.1: user subroutine matusr_24 in dyn21.f is called HR.EQ.7: Load curve defining biaxial stress vs. biaxial strain for hardening rule, see discussion in the formulation section below for a definition. HR.NE.7: Ignored. HR.EQ.7: Load curve defining shear stress vs. shear strain for hardening, see discussion in the formulation section below for a definition. HR.NE.7: Ignored. LCBI LCSH Formulation: The effective plastic strain used in this model is defined to be plastic work equivalent. A consequence of this is that for parameters defined as functions of effective plastic strain, the rolling (00) direction should be used as reference direction. For instance, the hardening curve for HR = 3 is the stress as function of strain for uniaxial tension in the rolling direction, VLCID curve should give the relative volume change as function of strain for uniaxial tension in the rolling direction and load curve given by -E should give the Young’s modulus as function of strain for uniaxial tension in the rolling direction. Optionally, the curve can be substituted for a table defining hardening as function of plastic strain rate (HR = 3) or temperature (HR = 8). Exceptions from the rule above are curves defined as functions of plastic strain in the 45 and 90 directions, i.e., P1 and P2 for HR = 7 and negative R45 or R90, see Fleischer et.al. [2007]. The hardening curves are here defined as measured stress as function of measured plastic strain for uniaxial tension in the direction of interest, i.e., as determined from experimental testing using a standard procedure. The optional biaxial and shear hardening curves require some further elaboration, as we assume that a biaxial or shear test reveals that the true stress tensor in the material system expressed as is a function of the (plastic) strain tensor 𝝈 = ( 0 ±𝜎 ) , 𝜎 ≥ 0, 𝜺 = ( 𝜀1 0 ±𝜀2 ) , 𝜀1 ≥ 0, 𝜀2 ≥ 0, The input hardening curves are 𝜎 as function of 𝜀1+𝜀2. The ± sign above distinguishes between the biaxial (+) and the shear (−) cases. Moreover, the curves defining the R values are as function of the measured plastic strain for uniaxial tension in the direction of interest. These curves are transformed internally to be used with the effective stress and strain properties in the actual model. The effective plastic strain does not coincide with the plastic strain components in other directions than the rolling direction and may be somewhat confusing to the user. Therefore the von Mises work equivalent plastic strain is output as history variable #2 if HR = 7 or if any of the R-values is defined as function of the plastic strain. The R-values in curves are defined as the ratio of instantaneous width change to instantaneous thickness change. That is, assume that the width W and thickness T are measured as function of strain. Then the corresponding R-value is given by: 𝑅 = 𝑑𝑊 𝑑𝜀 𝑑𝑇 𝑑𝜀 /𝑊 /𝑇 The anisotropic yield criterion Φ for plane stress is defined as: 𝑚 Φ = 𝑎|𝐾1 + 𝐾2|𝑚 + 𝑎|𝐾1 − 𝐾2|𝑚 + 𝑐|2𝐾2|𝑚 = 2𝜎𝑌 where 𝜎𝑌 is the yield stress and Ki = 1,2 are given by: 𝐾1 = 𝜎𝑥 + ℎ𝜎𝑦 √ √√ ⎷ 𝐾2 = ( 𝜎𝑥 − ℎ𝜎𝑦 ) 2 + 𝑝2𝜏𝑥𝑦 If PB = 0, the anisotropic material constants a, c, h, and p are obtained through R00, R45, and R90: 𝑎 = 2 − 2√( 𝑅00 1 + 𝑅00 ) ( 𝑅90 1 + 𝑅90 ) 𝑐 = 2 − 𝑎 ℎ = √( 𝑅00 1 + 𝑅00 ) ( 1 + 𝑅90 𝑅90 ) The anisotropy parameter p is calculated implicitly. According to Barlat and Lian the R value, width to thickness strain ratio, for any angle 𝜙 can be calculated from: 𝑅𝜙 = 2𝑚𝜎𝑌 + ∂Φ ∂𝜎𝑦 (∂Φ ∂𝜎𝑥 ) 𝜎𝜙 − 1 where 𝜎𝜙 is the uniaxial tension in the 𝜙 direction. This expression can be used to iteratively calculate the value of p. Let 𝜙 = 45 and define a function 𝑔 as: 𝑔(𝑝) = 2𝑚𝜎𝑌 + ∂Φ ∂𝜎𝑦 (∂Φ ∂𝜎𝑥 ) 𝜎𝜙 − 1 − 𝑅45 An iterative search is used to find the value of p. If PB > 0, material parameters a (AB), c (CB), h (HB), and p (PB) are used directly. For face centered cubic (FCC) materials m = 8 is recommended and for body centered cubic (BCC) materials m = 6 may be used. The yield strength of the material can be expressed in terms of k and n: 𝜎𝑦 = 𝑘𝜀𝑛 = 𝑘(𝜀𝑦𝑝 + 𝜀̅𝑝) where 𝜀𝑦𝑝 is the elastic strain to yield and 𝜀̅𝑝is the effective plastic strain (logarithmic). If SIGY is set to zero, the strain to yield if found by solving for the intersection of the linearly elastic loading equation with the strain hardening equation: 𝜎 = 𝐸𝜀 𝜎 = 𝑘𝜀𝑛 which gives the elastic strain at yield as: If SIGY yield is nonzero and greater than 0.02 then: 𝜀𝑦𝑝 = ( 𝑛−1 ) 𝜀𝑦𝑝 = ( 𝜎𝑦 ) The other available hardening models include the Voce equation given by: the Gosh equation given by: 𝜎Y(𝜀𝑝) = 𝑎 − 𝑏𝑒−𝑐𝜀𝑝, 𝜎Y(𝜀𝑝) = 𝑘(𝜀0 + 𝜀𝑝)𝑛 − 𝑝, and finally the Hocket-Sherby equation given by: 𝜎Y(𝜀𝑝) = 𝑎 − 𝑏𝑒−𝑐𝜀𝑝 . For the Gosh hardening law, the interpretation of the variable SPI is the same, i.e., if set to zero the strain at yield is determined implicitly from the intersection of the strain hardening equation with the linear elastic equation. To include strain rate effects in the model we multiply the yield stress by a factor depending on the effective plastic strain rate. We use the Cowper-Symonds’ model, hence the yield stress can be written as: 1/𝑝 𝜀̇𝑝 1 + ( 𝑠 (𝜀𝑝) 𝜎Y(𝜀𝑝, 𝜀̇𝑝) = 𝜎Y {⎧ ⎩{⎨ 𝑠 denotes the static yield stress, 𝐶 and 𝑝 are material parameters, 𝜀̇𝑝 is the where 𝜎Y effective plastic strain rate. It is also possible to use a table with HR.EQ.3 for defining the strain rate effects, for which each load curve in the table defines the yield stress as function of plastic strain for a given strain rate. In contrast to material 24, whenever the strain rate is higher than that of any curve in the table, the table is extrapolated in the strain rate direction to find the appropriate yield stress. }⎫ ⎭}⎬ ) A kinematic hardening model is implemented following the works of Chaboche and Roussilier. A back stress α is introduced such that the effective stress is computed as: 𝜎eff = 𝜎eff(𝜎11 − 2𝛼11 − 𝛼22, 𝜎22 − 2𝛼22 − 𝛼11, 𝜎12 − 𝛼12) The back stress is the sum of up to four terms according to: 𝛼𝑖𝑗 = ∑ 𝛼𝑖𝑗 𝑘=1 and the evolution of each back stress component is as follows: 𝛿𝛼𝑖𝑗 𝑘 = 𝐶𝑘 (𝑎𝑘 𝑠𝑖𝑗 𝜎eff − 𝛼𝑖𝑗 𝑘 ) 𝛿𝜀𝑝 where 𝐶𝑘 and 𝑎𝑘 are material parameters,𝑠𝑖𝑗 is the deviatoric stress tensor, 𝜎eff is the effective stress and 𝜀𝑝 is the effective plastic strain. The yield condition is for this case modified according to 𝑓 (σ,α, 𝜀𝑝) = 𝜎eff(𝜎11 − 2𝛼11 − 𝛼22, 𝜎22 − 2𝛼22 − 𝛼11, 𝜎12 − 𝛼12) − {𝜎𝑌 𝑡 (𝜀𝑝, 𝜀̇𝑝, 0) − ∑ 𝑎𝑘[1 − exp(−𝐶𝑘𝜀𝑝 ] } ≤ 0 in order to get the expected stress strain response for uniaxial stress. The calculated effective stress is stored in history variable #7. 𝑘=1 A Failure Criterion For Nonlinear Strain Paths (NLP) in sheet metal forming: When the option NLP is used, a necking failure criterion is activated to account for the non-linear strain path effect in sheet metal forming. Based on the traditional Forming Limit Diagram (FLD) for the linear strain path, the Formability Index (F.I.) is calculated for every element in the model throughout the simulation duration. The entire F.I. time history for every element is stored in history variable #1 in d3plot files, accessible from Post/History menu in LS-PrePost v4.0. In addition to the F.I. output, other useful information stored in other history variables can be found as follows, 1. Formability Index: #1 2. Strain ratio (in-plane minor strain/major strain): #2 3. Effective strain from the planar isotropic assumption: #3 To enable the output of these history variables to the d3plot files, NEIPS on the *DATA- BASE_EXTENT_BINARY card must be set to at least 3. The history variables can also be plotted on the formed sheet blank as a color contour map, accessible from Post/FriComp/Misc menu. The index value starts from 0.0, with the onset of necking failure when it reaches 1.0. The F.I. is calculated based on critical effect strain method, as illustrated in a figure in Remarks section in *MAT_037. The theoretical background can be found in two papers also referenced in Remarks section in *MAT_037. When d3plot files are used to plot the history variable #1 (the F.I.) in color contour, the value in the “Max” pull-down menu in Post/FriComp needs to be set to “Min”, meaning that the necking failure occurs only when all integration points through the thickness have reached the critical value of 1.0 (refer to Tharrett and Stoughton’s paper in 2003 SAE 2003-01-1157). It is also suggested to set the variable “MAXINT” in *DATABASE_EX- TENT_BINARY to the same value as the variable “NIP” in *SECTION_SHELL. In addition, the value in the “Avg” pull-down menu in Post/FriRang needs to be set to “None”. The strain path history (major vs. minor strain) of each element can be plotted with the radial dial button Strain Path in Post/FLD. An example of a partial input for the material is provided below, where the FLD for the linear strain path is defined by the variable NLP with load curve ID 211, where abscissas represent minor strains and ordinates represent major strains. *MAT_3-PARAMETER_BARLAT_NLP $---+----1----+----2----+----3----+----4----+----5----+----6----+----7----+----8 $ MID RO E PR HR P1 P2 ITER 1 2.890E-09 6.900E04 0.330 3.000 $ M R00 R45 R90 LCID E0 SPI P3 8.000 0.800 0.600 0.550 99 $ AOPT C P VLCID NLP 2.000 211 $ A1 A2 A3 0.000 1.000 0.000 $ V1 V2 V3 D1 D2 D3 BETA $---+----1----+----2----+----3----+----4----+----5----+----6----+----7----+----8 $ Hardening Curve *DEFINE_CURVE 99 0.000 130.000 0.002 134.400 0.006 143.000 0.010 151.300 0.014 159.300 ⋮ ⋮ 0.900 365.000 1.000 365.000 $ FLD Definition *DEFINE_CURVE 211 -0.2 0.325 -0.1054 0.2955 -0.0513 0.2585 0.0000 0.2054 0.0488 0.2240 0.0953 0.2396 0.1398 0.2523 0.1823 0.2622 ⋮ ⋮ Shown in Figures M36-1, M36-2 and M36-3, predictions and validations of forming limit curves (FLC) of various nonlinear strain paths on a single shell element was done using this new option, for an Aluminum alloy with r00 = 0.8, r45 = 0.6, r90 = 0.55, and yield at 130.0 MPa. In each case, the element is further strained in three different paths (uniaxial stress – U.A., plane strain – P.S., and equi-biaxial strain – E.B.) separately, following a pre-straining in uniaxial, plane strain and equi-biaxial strain state, respectively. The forming limits are determined at the end of the secondary straining for each path, when the F.I. has reached the value of 1.0. It is seen that the predicted FLCs (dashed curves) in case of the nonlinear strain paths are totally different from the FLCs under the linear strain paths. It is noted that the current predicted FLCs under nonlinear strain path are obtained by connecting the ends of the three distinctive strain paths. More detailed FLCs can be obtained by straining the elements in more paths between U.A. and P.S. and between P.S. and E.B. In Figure M36-4, time-history plots of F.I., strain ratio and effective strain are shown for uniaxial pre-strain followed by equi-biaxial strain path on the same single element. Typically, to assess sheet formability, F.I. contour of the entire part should be plotted. Based on the contour plot, non-linear strain path and the F.I. time history of a few elements in the area of concern can be plotted for further study. These plots are similar to those shown in manual pages of *MAT_037. Heat treatment with variable HTFLAG: Heat treatment for increasing the formability of prestrained aluminum sheets can be simulated through the use of HTFLAG, where the intention is to run a forming simulation in steps involving preforming, springback, heat treatment and postforming. In each step the history is transferred to the next via the use of dynain . The first two steps are performed with HTFLAG = 0 according 0corresponding to the to standard procedures, resulting in a plastic strain field 𝜀𝑝 prestrain. The heat treatment step is performed using HTFLAG = 1 in a coupled thermomechanical simulation, where the blank is heated. The coupling between thermal and mechanical is only that the maximum temperature 𝑇0 is stored as a history variable in the material model, this corresponding to the heat treatment temperature. Here it is important to export all history variables to the dynein file for the postforming step. In the final postforming step, HTFLAG = 2, the yield stress is then augmented by the Hocket-Sherby like term: 0) Δ𝜎 = 𝑏 − (𝑏 − 𝑎)exp[−𝑐(𝜀𝑝 − 𝜀𝑝 ] where a, b, c and d are given as tables as functions of the heat treatment temperature 𝑇0 0. That is, in the table definitions each load curve corresponds to a given and prestrain 𝜀𝑝 prestrain and the load curve value is with respect to the heat treatment temperature, 𝑎 = 𝑎(𝑇0, 𝜀𝑝 0) 𝑏 = 𝑏(𝑇0, 𝜀𝑝 0) 𝑐 = 𝑐(𝑇0, 𝜀𝑝 0) 𝑑 = 𝑑(𝑇0, 𝜀𝑝 0) The effect of heat treatment is that the material strength decreases but hardening increases, thus typically: 𝑎 ≤ 0 𝑏 ≥ 𝑎 𝑐 > 0 𝑑 > 0 Revision information: The option NLP is available in explicit dynamic analysis and in SMP and MPP, starting in Revision 95576. Fx 0= n i- a x i a l str e s s Fx 0= uy P la n e str ai n uy Fx 0= n i- a x i a l str e s s Fx 0= uy u i- b ia x ial uy ux uy= n str a i n e ll s h FLC- nonlinear strain path FLC- linear strain path 0.35 0.30 0.25 0.20 0.15 0.10 0.05 U.A. P.S. E.B. U.A. -0.2 -0.1 0.1 Minor true strain 0.2 Figure M36-1. Nonlinear FLD prediction with uniaxial pre-straining. Fx 0= n i- a x i a l str e s s Fx 0= uy P la n e str ai n uy P la n e str ai n uy u i- b ia x ial uy ux uy= n str a i n e ll s h FLC- nonlinear strain path FLC- linear strain path 0.35 0.30 0.25 0.20 0.15 0.10 0.05 U.A. P.S. E.B. P.S. -0.2 -0.1 0.1 Minor true strain 0.2 Figure M36-2. Nonlinear FLD prediction with plane strain pre-straining. Fx 0= n i- a x i a l str e s s Fx 0= uy P la n e str ai n u i- b ia x ial uy ux uy= uy u i- b ia x ial uy ux uy= n str a i n e ll s h FLC- nonlinear strain path FLC- linear strain path U.A. E.B. P.S. E.B. 0.35 0.30 0.25 0.20 0.15 0.10 0.05 -0.2 -0.1 0.1 Minor true strain 0.2 Figure M36-3. Nonlinear FLD prediction with equi-biaxial pre-straining. 1.2 1.0 0.8 0.6 0.4 0.2 0.0 1.0 0.8 0.6 0.4 0.2 0.0 -0.2 -0.4 0.6 0.5 0.4 0.3 0.2 0.1 0.0 ) # ( . . ) # ( ) # ( Uniaxial Equi-biaxial Time, seconds (E-03) Uniaxial Equi-biaxial Time, seconds (E-03) Uniaxial Equi-biaxial Time, seconds (E-03) Figure M36-4. Time-history plots of the three history variables. *MAT_EXTENDED_3-PARAMETER_BARLAT This is Material Type 36E. This model is an extension to the standard 3-parameter Barlat model and allows for different hardening curves and R-values in different directions, see Fleischer et.al. [2007]. The directions in this context are the three uniaxial directions (0, 45 and 90 degrees) and optionally biaxial and shear. Card 1 1 Variable MID Type A8 Card 2 1 2 RO F 2 3 E F 3 4 PR F 4 5 6 7 8 5 6 7 8 Variable LCH00 LCH45 LCH90 LCHBI LCHSH Type F Card 3 1 F 2 F 3 F 4 F 5 Variable LCR00 LCR45 LCR90 LCRBI LCRSH F 2 F 3 Type F Card 4 1 Variable AOPT Type F Card 5 1 2 3 Variable Type 2-270 (EOS) F 4 4 A1 F F 5 5 A2 F 6 M F 6 6 A3 F 7 8 7 8 Card 6 Variable 1 V1 Type F 2 V2 F 3 V3 F 4 D1 F 5 D2 F 6 D3 F 7 8 BETA F VARIABLE DESCRIPTION MID RO E PR LCHXX LCHBI LCHSH LCRXX LCRBI Material identification. A unique number or label not exceeding 8 characters must be specified. Mass density. Young’s modulus, 𝐸. Poisson’s ratio, ν. Load curve defining uniaxial stress vs. uniaxial strain in the given direction (XX is either 00, 45, 90). The exact definition is discussed in the Remarks below. LCH00 must be defined, the other defaults to LCH00 if not defined. Load curve defining biaxial stress vs. biaxial strain, see discussion in the Remarks below for a definition. If not defined this is determined from LCH00 and the initial R-values to yield a response close to the standard 3-parameter Barlat model. Load curve defining shear stress vs. shear strain, see discussion in the Remarks below for a definition. If not defined this is ignored to yield a response close to the standard 3-parameter Barlat model. Load curve defining standard R-value vs. uniaxial strain in the given direction (XX is either 00, 45, 90). The exact definition is discussed in the Remarks below. Default is a constant R-value of 1.0, a negative input will result in a constant R-value of –LCRXX. Load curve defining biaxial R-value vs. biaxial strain, see discussion in the Remarks below for a definition. Default is a constant R-value of 1.0, a negative input will result in a constant R-value of –LCRBI. LCRSH M AOPT *MAT_EXTENDED_3-PARAMETER_BARLAT DESCRIPTION Load curve defining shear R-value vs. shear strain, see discussion in the Remarks below for a definition. Default is a constant R- value of 1.0, a negative input will result in a constant R-value of – LCRSH. Barlat flow exponent, 𝑚, must be an integer value. Material axes option : EQ.0.0: locally orthotropic with material axes determined by element nodes 1, 2, and 4, as with *DEFINE_COORDI- NATE_NODES, and then rotated about the shell ele- ment normal by an angle BETA. EQ.2.0: globally orthotropic with material axes determined by vectors defined below, as with *DEFINE_COORDI- NATE_VECTOR. EQ.3.0: locally orthotropic material axes determined by rotating the material axes about the element normal by an angle, BETA, from a line in the plane of the element defined by the cross product of the vector v with the element normal. LT.0.0: the absolute value of AOPT is a coordinate system ID number (CID on *DEFINE_COORDINATE_NODES, *DEFINE_COORDINATE_SYSTEM or *DEFINE_CO- ORDINATE_VECTOR). Available with the R3 release of Version 971 and later. XP, YP, ZP Coordinates of point 𝐩 for AOPT = 1. A1, A2, A3 Components of vector 𝐚 for AOPT = 2. V1, V2, V3 Components of vector 𝐯 for AOPT = 3. D1, D2, D3 Components of vector 𝐝 for AOPT = 2. BETA Material angle in degrees for AOPT = 0 and 3, may be overridden on the element card, see *ELEMENT_SHELL_BETA. Formulation: The hardening curves LCH00, LCH45 and LCH90 are here defined as measured stress as function of measured plastic strain for uniaxial tension in the direction of interest, i.e., as determined from experimental testing using a standard procedure. The optional biaxial and shear hardening curves LCHBI and LCHSH require some further elaboration, as we assume that a biaxial or shear test reveals that the true stress tensor in the material system expressed as is a function of the (plastic) strain tensor 𝝈 = ( 0 ±𝜎 ) , 𝜎 ≥ 0, 𝜺 = ( 𝜀1 0 ±𝜀2 ) , 𝜀1 ≥ 0, 𝜀2 ≥ 0, The input hardening curves are 𝜎 as function of 𝜀1+𝜀2. The ± sign above distinguishes between the biaxial (+) and the shear (−) cases. Moreover, the curves LCR00, LCR45 and LCR90 defining the R values are as function of the measured plastic strain for uniaxial tension in the direction of interest. The R-values in themselves are defined as the ratio of instantaneous width change to instantaneous thickness change. That is, assume that the width W and thickness T are measured as function of strain. Then the corresponding R-value is given by: 𝑅𝜑 = 𝑑𝑊 𝑑𝜀 𝑑𝑇 𝑑𝜀 /𝑊 /𝑇 . These curves are transformed internally to be used with the effective stress and strain properties in the actual model. The effective plastic strain does not coincide with the plastic strain components in other directions than the rolling direction and may be somewhat confusing to the user. Therefore the von Mises work equivalent plastic strain is output as history variable #2. As for hardening, the optional biaxial and shear R- value curves LCRBI and LCRSH are defined in a special way for which we return to the local plastic strain tensor 𝜺 as defined above. The biaxial and shear R-values are defined as 𝑅𝑏/𝑠 = 𝜀̇1 𝜀̇2 and again the curves are 𝑅𝑏/𝑠 as function of 𝜀1+𝜀2. Note here that the suffix 𝑏 assumes loading biaxially and 𝑠 assumes loading in shear, so the R-values to be defined are always positive. *MAT_TRANSVERSELY_ANISOTROPIC_ELASTIC_PLASTIC_{OPTION} This is Material Type 37. This model is for simulating sheet forming processes with anisotropic material. Only transverse anisotropy can be considered. Optionally an arbitrary dependency of stress and effective plastic strain can be defined via a load curve. This plasticity model is fully iterative and is available only for shell elements. Available options include: <BLANK> ECHANGE NLP_FAILURE NLP2 The ECHANGE option allows the change of Young’s Modulus during the simulation: The NLP_FAILURE option estimates failure using the Formability Index (F.I.) which accounts for the non-linear strain paths common in metal forming application . The option NLP is also available in *MAT_036, *MAT_125 and *MAT_226. The NLP_FAULURE option uses effective plastic strain to calculate the onset of necking, which assumes the necking happens in an instant. Some researchers think it may happen in a longer duration, which can be addressed by the option NLP2, which calculates the damage during forming and accumulates it to predict the sheet metal failure. Compared with NLP_FAILURE, there is no input change required. Card 1 1 Variable MID Type A 2 RO F 3 E F 4 PR F 5 6 SIGY ETAN F F 7 R F 8 HLCID F Additional card for ECHANGE and/or NLP_FAILURE keyword options. Card 2. 1 Variable IDSCALE Type I 2 EA F 3 4 5 6 7 8 COE ICFLD STRAINLT F F VARIABLE DESCRIPTION MID RO E PR SIGY ETAN Material identification. A unique number or label not exceeding 8 characters must be specified. Mass density. Young’s modulus. Poisson’s ratio. Yield stress. Plastic hardening modulus. When this value is negative, normal stresses (either from contact or applied pressure) are considered and *LOAD_SURFACE_STRESS must be used to capture the stresses. The negative local 𝑧-stresses caused by the contact pressure can be viewed from d3plot files after Revision 97158. This data can be viewed in LS-PrePost by selecting 𝑧-stress under FCOMP → Stress and select local under FCOMP in LS-PrePost). Prior to Revision 97158, the negative local 𝑧-stresses are stored in history variable #5, and can be viewed with menu options FCOMP → Misc → history var #5 in LS-PrePost. This feature is applicable to both shell element types 2 and 16. It is found in some cases this inclusion can improve forming simulation accuracy. R Anisotropic parameter, also commonly call r-bar, 𝑟 ̅, in sheet metal forming literature. Its interpretation is given here. GT.0: Standard formulation. LT.0: The anisotropic parameter is set to |R|. When R is set to a negative value the algorithm is modified for better sta- bility in sheet thickness or thinning for sheet metal form- ing involving high strength steels or in cases when the simulation time is long. This feature is available to both element formulations 2 and 16. An example using this feature is provided in Remarks, and shown in Figure M37-4. HLCID Load curve ID expressing effective yield stress as a function of effective plastic strain in uniaxial tension. IDSCALE EA, COE ICFLD *MAT_TRANSVERSELY_ANISOTROPIC_ELASTIC_PLASTIC DESCRIPTION Load curve ID expressing the scale factor for the Young’s modulus as a function of effective strain. If the EA and COE fields are specified, this curve is unnecessary. This field is only used and should only be specified when the option ECHANGE is active. Coefficients defining the Young’s modulus with respect to the effective strain, EA is 𝐸𝐴 and COE is 𝜁 . If IDSCALE is defined, these two parameters are not necessary. Input only when the option ECHANGE is used. Also see *MAT_125 for an example to obtain these two coefficients from a test curve. ID of a load curve of the Forming Limit Diagram (FLD) under linear strain paths . In the load curve, abscissas represent minor strains while ordinates represent major strains. Define only when the option NLP_FAILURE is active. STRAINLT Critical strain value at which strain averaging is activated. Input only when the option NLP_FAILURE is active. See Remarks. Formulation: Consider Cartesian reference axes which are parallel to the three symmetry planes of anisotropic behavior. Then, the yield function suggested by Hill [1948] can be written as: 𝐹(𝜎22 − 𝜎33)2 + 𝐺(𝜎33 − 𝜎11)2 + 𝐻(𝜎11 − 𝜎22)2 + 2𝐿𝜎23 2 + 2𝑀𝜎31 2 + 2𝑁𝜎12 2 − 1 = 0 where 𝜎𝑦1, 𝜎𝑦2, and 𝜎𝑦3, are the tensile yield stresses and 𝜎𝑦12, 𝜎𝑦23, and 𝜎𝑦31 are the shear yield stresses. The constants F, G H, L, M, and N are related to the yield stress by: 2𝐿 = 2𝑀 = 2𝑁 = 2 𝜎𝑦23 2 𝜎𝑦31 2 𝜎𝑦12 2𝐹 = 2 + 𝜎𝑦2 2 − 𝜎𝑦3 2 𝜎𝑦1 2𝐺 = 2 + 𝜎𝑦3 2 − 𝜎𝑦1 2 𝜎𝑦2 2𝐻 = 2 + 𝜎𝑦1 2 − 𝜎𝑦2 2 . 𝜎𝑦3 The isotropic case of von Mises plasticity can be recovered by setting: and 𝐹 = 𝐺 = 𝐻 = 𝐿 = 𝑀 = 𝑁 = 2 2𝜎𝑦 2 2𝜎𝑦 For the particular case of transverse anisotropy, where properties do not vary in the x1- x2 plane, the following relations hold: 2𝐹 = 2𝐺 = 2 𝜎𝑦3 2𝐻 = 2 − 𝜎𝑦 2 𝜎𝑦3 𝑁 = 2 − 𝜎𝑦 2 𝜎𝑦3 where it has been assumed that 𝜎𝑦1 = 𝜎𝑦2 = 𝜎𝑦. Letting 𝐾 = 𝜎𝑦 𝜎𝑦3 , the yield criteria can be written as: 𝐹(𝜎) = 𝜎𝑒 = 𝜎𝑦, where, 𝐹(𝜎) ≡ [𝜎11 2 + 𝜎22 2 + 𝐾2𝜎33 2 − 𝐾2𝜎33(𝜎11 + 𝜎22) − (2 − 𝐾2)𝜎11𝜎22 + 2𝐿𝜎𝑦 2(𝜎23 2 ) 2 + 𝜎31 + 2 (2 − 2 ] 𝐾2) 𝜎12 2⁄ . The rate of plastic strain is assumed to be normal to the yield surface so 𝜀̇𝑖𝑗 from: 𝑝 is found 𝑝 = 𝜆 𝜀̇𝑖𝑗 ∂𝐹 ∂𝜎𝑖𝑗 . Now consider the case of plane stress, where σ33 = 0. Also, define the anisotropy input parameter, R, as the ratio of the in-plane plastic strain rate to the out-of-plane plastic strain rate, 𝑅 = 𝜀̇22 𝑝 . 𝜀̇33 It then follows that 𝑅 = 𝐾2 − 1. Using the plane stress assumption and the definition of R, the yield function may now be written as: 𝐹(𝜎) = [𝜎11 2 + 𝜎22 2 − 2𝑅 𝑅 + 1 𝜎11𝜎22 + 2 2𝑅 + 1 𝑅 + 1 2⁄ . 2 ] 𝜎12 Discussion and ECHANGE: It is noted that there are several differences between this model and other plasticity models for shell elements such as the model, MAT_PIECEWISE_LINEAR_PLASTICI- TY. First, the yield function for plane stress does not include the transverse shear stress components which are updated elastically, and, secondly, this model is always fully iterative. Consequently, in comparing results for the isotropic case where R = 1.0 with other isotropic model, differences in the results are expected, even though they are usually insignificant. The Young’s modulus has been assumed to be constant. Recently, some researchers have found that Young’s modulus decreases with respect to the increase of effective strain. To accommodate this new observation, a new option of ECHANGE is added. There are two methods defining the change of Young’s modulus change: The first method is to use a curve to define the scale factor with respect to the effective strain. The value of this scale factor should decrease from 1 to 0 with the increase of effective strain. The second method is to use a function as proposed by Yoshida [2003]: 𝐸 = 𝐸0 − (𝐸0 − 𝐸𝐴)[1 − exp(−𝜁 𝜀)]. An example of the option ECHANGE is provided in the Remarks section of the *MAT_- 125 manual pages. A Failure Criterion for Nonlinear Strain Paths (NLP): Background and Definition. When the option NLP_FAILURE is used, a necking failure criterion independent of strain path changes is activated. In sheet metal forming, as strain path history (plotted on in-plane major and minor strain space) of an element becomes non-linear, the position and shape of a traditional strain-based Forming Limit Diagram (FLD) changes. This option provides a simple formability index (F.I.) which remains invariant regardless of the presence of the non-linear strain paths in the model, and can be used to identify if the element has reached its necking limit. 0.4 0.3 0.2 0.1 -0.5 F.I. = Y / YL YL 0.1 1.0 β = dε2 / dε1 Figure M37-1. Calculation of F.I. based on critical effective strain method. Formability index (F.I) is calculated, as illustrated in Figure M37-1, for every element in the sheet blank throughout the simulation duration. The value of F.I. is 0.0 for virgin material and reaches maximum of 1.0 when the material fails. The theoretical background can be found in two papers: 1) T.B. Stoughton, X. Zhu, “Review of Theoretical Models of the Strain-Based FLD and their Relevance to the Stress-Based FLD, International Journal of Plasticity”, V. 20, Issues 8-9, P. 1463-1486, 2003; and 2) Danielle Zeng, Xinhai Zhu, Laurent B. Chappuis, Z. Cedric Xia, “A Path Independent Forming Limited Criterion for Sheet Metal Forming Simulations”, 2008 SAE Proceedings, Detroit MI, April, 2008. Required inputs. The load curve input for ICFLD follows keyword format in *DEFINE_CURVE, with abscissas as minor strains and ordinates as major strains. ICFLD can also be specified using the *DEFINE_CURVE_FLC keyword where the sheet metal thickness and strain hardening value are used. Detailed usage information can be found in the manual entry for *DEFINE_CURVE_FLC. The formability index is output as a history variable #1 in d3plot files. In addition to the F.I. values, starting in Revision 95599, the strain ratio 𝛽 and effective plastic strain 𝜀̅ are written to the d3plot database as history variables #2 and #3, respectively provided NEIPS on the second field of the first card of *DATABASE_EXTENT_BINARY is set to at least 3. The contour map of history variables can be plotted in LS-PrePost, accessible in Post/FriComp, under Misc, and by Element, under Post/History. Post-processing information. When plotting the formability index contour map, first select the history var #1 from Misc in the FriComp menu. The pull-down menu under FriComp can be used to select the minimum value “Min” for necking failure detection (refer to Tharrett and Stoughton’s paper in 2003 SAE 2003-01-1157). In the FriRang dialog, select None on the pull-down menu next to “Avg”. Lastly, set the simulation result to the last state on the animation tool bar. The index value ranges from 0.0 to 1.5. The non-linear forming limit is reached at 1.0. In addition, the evolution of the index throughout the simulation can be plotted in LS- PrePost4.0 under Post/History by Element. Select the last entry, which is history var#1 it may be hidden by a scroll bar. Furthermore, the strain path of an element can be plotted in Post/FLD, using the Tracer option, by selecting the corresponding integration point representing the “Min” index value in the Position pull-down menu. Similarly contour maps and the evolution of the strain ratio and the effective plastic strain can be plotted in the same way using variables 2 and 3. By setting the STRAINLT field strains (and strain ratios) can be averaged to reduce noise, which, in turn, affect the calculation of the formability index. The strain STRAINLT causes the formability index calculation to use only time averaged strains. Reasonable STRAINLT values range from 5 × 10−3 to 10−2. It is suggested that variable “MAXINT” in *DATABASE_EXTENT_BINARY be set to the same value of as the “NIP” field for the *SECTION_SHELL keyword. Input example. An example of a partial keyword input using this non-linear strain path failure criterion is provided below: *KEYWORD ... *DATABASE_EXTENT_BINARY $ NEIPH NEIPS MAXINT STRFLG SIGFLG EPSFLG RLTFLG ENGFLG 3 &nip 1 $ CMPFLG IEVERP BEAMIP DCOMP SHGE STSSZ 1 2 ... *MAT_TRANSVERSELY_ANISOTROPIC_ELASTIC_PLASTIC_NLP_FAILURE $ MID RO E PR SIGY ETAN R HLCID 1 7.830E-09 2.070E+05 0.28 0.0 0.0 0.864 200 $ IDY EA COE ICFLD STRAINLT 891 1.0E-02 *DEFINE_CURVE 891 $ minor, major strains for FLD definition -3.375000e-01 4.965000e-01 -2.750000e-01 4.340000e-01 -2.250000e-01 3.840000e-01 -1.840909e-01 3.430909e-01 -1.500000e-01 3.090000e-01 -1.211539e-01 2.801539e-01 -9.642858e-02 2.554286e-01 -7.500000e-02 2.340000e-01 -5.625001e-02 2.152500e-01 -3.970589e-02 1.987059e-01 -2.500000e-02 1.840000e-01 $$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ $ load curve 200: Mat_037 property, DP600 NUMISHEET'05 Xmbr, Power law fit $$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ *DEFINE_CURVE 200 0.000,395.000 0.001,425.200 0.003,440.300 0.004,452.000 0.005,462.400 0.006,472.100 As shown in Figure M37-2, F.I contours can be plotted using FriComp/Misc, in LS- PrePost4.0. Strain paths of individual elements, or elements in an area can be plotted (Figure M37-3 left) using the “Tracer” feature in the FLD menu. Finally, time history plot of the formability index for elements selected can be plotted in History menu, Figure M37-3 right. Thickness/Thinning Stabilization for Shell Types 2 and 16: When the 𝑅 value is set to a negative value, it stabilizes the sheet thickness or thinning in sheet metal forming for some high strength types of steel or in cases where the simulation time is long. In Figure M37-4, a comparison of thinning contours is shown on a U-channel forming (one-half model) using negative and positive R values. Maximum thinning on the draw wall is slight higher in the negative R case than that in the positive R case. Revision information: 1)The NLP_FAILURE option is implemented in explicit dynamic and is available starting in Revision 60925. 2)The maximum F.I. value is change from 1.0 to 1.5 starting in Revision 72219. 3)The NLP_FAILURE option is also available starting in Revision 73241 for implicit static calculation. 4)History variables #2 and #3 output is available starting in Revision 95599. in d3plot 5)Local *LOAD_SURFACE_STRESS) is available starting in Revision 97158. stress output (when used files 𝑧 together with 6)Negative 𝐸 option (contact pressure/normal stress) activated in formability index starts in Revision 97296. 7)Numerical material model type with the NLP_FAILURE option (*MAT_037_NLP_FAULURE) is available starting in Revision 106898. 8)Revision 111547: option NLP2. Time = 0.1587, #nodes=476931 Contours of History Variable#1 min. ipt. value min=0, at elem# 305 max=1, at elem# 8887 Formability Index 1.0 0.9 0.8 0.7 0.6 0.5 0.4 0.3 0.2 0.1 Figure M37-2. F.I. contour plot (min IP value, non-averaged). 0.60 0.50 0.40 0.30 0.20 0.10 -0.2 -0.1 0.1 Minor true strain 1.0 0.8 0.6 0.4 0.2 . # , # 0.05 0.1 0.15 Time (sec.) Nonlinear strain paths of a few elements in the box F.I. time history plots of the elements Figure M37-3. Strain paths and F.I. history plot for elements in the black square box of the previous Figure. Time=0.010271, #nodes=4594, #elem=4349 Contours of % Thickness Reduction based on current z-strain min=0.0093799, at elem#42249 max=22.1816, at elem#39875 Time=0.010271, #nodes=4594, #elem=4349 Contours of % Thickness Reduction based on current z-strain min=0.0597092, at elem#39814 max=21.2252, at elem#40457 Thinning % 20 18 16 14 12 10 With negative R-value With positive R-value Figure M37-4. Thinning contour comparison. *MAT_BLATZ-KO_FOAM *MAT_BLATZ-KO_FOAM *MAT_038 This is Material Type 38. This model is for the definition of rubber like foams of polyurethane. It is a simple one-parameter model with a fixed Poisson’s ratio of .25. Card 1 1 Variable MID 2 RO Type A8 F 3 G F 4 REF F 5 6 7 8 VARIABLE DESCRIPTION Material identification. A unique number or label not exceeding 8 characters must be specified. Mass density. Shear modulus. Use reference geometry to initialize the stress tensor. The reference geometry is defined by the keyword:*INITIAL_FOAM_- REFERENCE_GEOMETRY . EQ.0.0: off, EQ.1.0: on. MID RO G REF Remarks: The strain energy functional for the compressible foam model is given by 𝑊 = ( II III + 2√III − 5) Blatz and Ko [1962] suggested this form for a 47 percent volume polyurethane foam rubber with a Poisson’s ratio of 0.25. In terms of the strain invariants, I, II, and III, the second Piola-Kirchhoff stresses are given as 𝑆𝑖𝑗 = 𝐺 [(𝐼𝛿𝑖𝑗 − 𝐶𝑖𝑗) III + (√III − II III ) 𝐶𝑖𝑗 −1] where Cij is the right Cauchy-Green strain tensor. This stress measure is transformed to the Cauchy stress, σij, according to the relationship 𝜎 𝑖𝑗 = III −1 2⁄ 𝐹𝑖𝑘𝐹𝑗𝑙𝑆𝑙𝑘 where Fij is the deformation gradient tensor. *MAT_FLD_TRANSVERSELY_ANISOTROPIC This is Material Type 39. This model is for simulating sheet forming processes with anisotropic material. Only transverse anisotropy can be considered. Optionally, an arbitrary dependency of stress and effective plastic strain can be defined via a load curve. A Forming Limit Diagram (FLD) can be defined using a curve and is used to compute the maximum strain ratio which can be plotted in LS-PrePost. This plasticity model is fully iterative and is available only for shell elements. Also see the notes below. 2 RO F 2 3 E F 3 4 PR F 4 5 6 SIGY ETAN F 5 F 6 7 R F 7 8 HLCID F 8 Card 1 1 Variable MID Type A8 Card 2 1 Variable LCFLD Type F VARIABLE DESCRIPTION MID RO E PR SIGY ETAN Material identification. A unique number or label not exceeding 8 characters must be specified. Mass density. Young’s modulus. Poisson’s ratio. Yield stress. Plastic hardening modulus, see notes for model 37. R Anisotropic hardening parameter, see notes for model 37. HLCID Load curve ID defining effective stress versus effective plastic strain. The yield stress and hardening modulus are ignored with this option. mjr = 0 mjr Plane Strain 80 70 60 50 40 30 20 10 mnr mjr mnr Draw mjr Stretch % -50 -40 -30 -20 -10 10 20 30 40 50 % Minor Strain Figure M39-1. Forming limit diagram. DESCRIPTION Load curve ID defining the Forming Limit Diagram. Minor strains in percent are defined as abscissa values and Major strains in percent are defined as ordinate values. The forming limit diagram is shown in Figure M39-1. In defining the curve list pairs of minor and major strains starting with the left most point and ending with the right most point, see *DEFINE_CURVE. VARIABLE LCFLD Remarks: See material model 37 for the theoretical basis. The first history variable is the maximum strain ratio: 𝜀majorworkpiece 𝜀majorfld . corresponding to 𝜀minorworkpiece. *MAT_NONLINEAR_ORTHOTROPIC This is Material Type 40. This model allows the definition of an orthotropic nonlinear elastic material based on a finite strain formulation with the initial geometry as the reference. Failure is optional with two failure criteria available. Optionally, stiffness proportional damping can be defined. In the stress initialization phase, temperatures can be varied to impose the initial stresses. This model is only available for shell and solid elements. WARNING: We do not recommend using this model at this time since it can be unstable especially if the stress-strain curves increase in stiffness with in- creasing strain. Card 1 1 Variable MID 2 RO Type A8 F 3 EA F 4 EB F 5 EC F 6 7 8 PRBA PRCA PRCB F F F Default none none none none none none none none Card 2 1 2 3 Variable GAB GBC GCA Type F F F Default none none none 4 DT F 0 5 6 7 8 TRAMP ALPHA F 0 F Card 3 1 2 3 4 5 6 7 8 Variable LCIDA LCIDB EFAIL DTFAIL CDAMP AOPT MACF Type F F F F F F Default 0.0 0.0 0.0 0.0 0.0 0.0 Card 4 Variable 1 XP Type F Card 5 Variable 1 V1 Type F 2 YP F 2 V2 F 3 ZP F 3 V3 F 4 A1 F 4 D1 F 5 A2 F 5 D2 F 6 A3 F 6 D3 F I 0 7 8 7 8 BETA F Optional Card 6 (Applies to Solid elements only) Card 6 1 2 3 4 5 6 7 8 Variable LCIDC LCIDAB LCIDBC LCIDCA Type F F F F Default optional optional optional optional VARIABLE MID DESCRIPTION Material identification. A unique number or label not exceeding 8 characters must be specified. RO Mass density. VARIABLE DESCRIPTION EA EB EC PRBA PRCA PRCB GAB GBC GCA DT 𝐸𝑎, Young’s modulus in 𝑎-direction. 𝐸𝑏, Young’s modulus in 𝑏-direction. 𝐸𝑐, Young’s modulus in 𝑐-direction. 𝜈𝑏𝑎, Poisson’s ratio 𝑏𝑎. 𝜈𝑏𝑎, Poisson’s ratio 𝑐𝑎. 𝜈𝑐𝑏, Poisson’s ratio 𝑐𝑏. 𝐺𝑎𝑏, shear modulus 𝑎𝑏. 𝐺𝑏𝑐, shear modulus 𝑏𝑐. 𝐺𝑐𝑎, shear modulus 𝑐𝑎. Temperature increment for isotropic stress initialization. This option can be used during dynamic relaxation. TRAMP Time to ramp up to the final temperature. ALPHA Thermal expansion coefficient. LCIDA LCIDB Optional load curve ID defining the nominal stress versus strain along 𝑎-axis. Strain is defined as 𝜆𝑎 − 1 where 𝜆𝑎 is the stretch ratio along the 𝑎-axis. Optional load curve ID defining the nominal stress versus strain along 𝑏-axis. Strain is defined as 𝜆𝑏 − 1 where 𝜆𝑏 is the stretch ratio along the 𝑏-axis. EFAIL Failure strain, 𝜆 − 1. DTFAIL Time step for automatic element erosion CDAMP Damping coefficient. AOPT Material axes option : EQ.0.0: locally orthotropic with material axes determined by element nodes 1, 2, and 4, as with *DEFINE_COORDI- NATE_NODES, and then, for shells only, rotated about the shell element normal by an angle BETA. *MAT_NONLINEAR_ORTHOTROPIC DESCRIPTION EQ.1.0: locally orthotropic with material axes determined by a point in space and the global location of the element center; this is the 𝑎-direction. This option is for solid elements only. EQ.2.0: globally orthotropic with material axes determined by vectors defined below, as with *DEFINE_COORDI- NATE_VECTOR. EQ.3.0: locally orthotropic material axes determined by rotating the material axes about the element normal by an angle, BETA, from a line in the plane of the element defined by the cross product of the vector v with the element normal. The plane of a solid element is the midsurface between the inner surface and outer surface defined by the first four nodes and the last four nodes of the connectivity of the element, respectively. EQ.4.0: locally orthotropic in cylindrical coordinate system with the material axes determined by a vector 𝐯, and an originating point, 𝐩, which define the centerline ax- is. This option is for solid elements only. LT.0.0: the absolute value of AOPT is a coordinate system ID number (CID on *DEFINE_COORDINATE_NODES, *DEFINE_COORDINATE_SYSTEM or *DEFINE_CO- ORDINATE_VECTOR). Available in R3 version of 971 and later. MACF Material axes change flag: EQ.1: No change, default, EQ.2: switch material axes 𝑎 and 𝑏, EQ.3: switch material axes 𝑎 and 𝑐, EQ.4: switch material axes 𝑏 and 𝑐. XP, YP, ZP Define coordinates of point 𝐩 for AOPT = 1 and 4. A1, A2, A3 (𝑎1, 𝑎2, 𝑎3) define components of vector 𝐚 for AOPT = 2. D1, D2, D3 (𝑑1, 𝑑2, 𝑑3) define components of vector 𝐝 for AOPT = 2. V1, V2, V3 (𝑣1, 𝑣2, 𝑣3) define components of vector 𝐯 for AOPT = 3 and 4. VARIABLE BETA DESCRIPTION Material angle in degrees for AOPT = 0 (shells only) and AOPT = 3. BETA may be overridden on the element card, see *ELEMENT_SHELL_BETA and *ELEMENT_SOLID_ORTHO.. The following input is optional and applies to SOLID ELEMENTS only LCIDC LCIDAB LCIDBC LCIDCA Load curve ID defining the nominal stress versus strain along 𝑐- axis. Strain is defined as 𝜆𝑐 − 1 where 𝜆𝑐 is the stretch ratio along the 𝑐-axis. Load curve ID defining the nominal ab shear stress versus 𝑎𝑏- strain in the 𝑎𝑏-plane. Strain is defined as the sin(𝛾𝑎𝑏) where 𝛾𝑎𝑏 is the shear angle. Load curve ID defining the nominal ab shear stress versus 𝑎𝑏- strain in the 𝑏𝑐-plane. Strain is defined as the sin(𝛾𝑏𝑐)where 𝛾𝑏𝑐 is the shear angle. Load curve ID defining the nominal ab shear stress versus 𝑎𝑏- strain in the 𝑐𝑎-plane. Strain is defined as the sin(𝛾𝑐𝑎) where 𝛾𝑐𝑎 is the shear angle. *MAT_USER_DEFINED_MATERIAL_MODELS These are Material Types 41 - 50. The user must provide a material subroutine. See also Appendix A. This keyword input is used to define material properties for the subroutine. Isotopic, anisotropic, thermal, and hyperelastic material models with failure can be handled. Card 1 1 2 3 4 5 6 7 Variable MID RO MT LMC NHV IORTHO/ ISPOT IBULK Type A8 Card 2 1 F 2 I 3 I 4 I 5 I 6 Variable IVECT IFAIL ITHERM IHYPER IEOS LMCA Type I I I I I I Additional card for IORTHO = 1. Card 3 1 2 Variable AOPT MACF Type F I Card 4 Variable 1 V1 Type F 2 V2 F 3 XP F 3 V3 F 4 YP F 4 D1 F 5 ZP F 5 D2 F 6 A1 F 6 D3 F I 7 7 A2 F 7 8 IG I 8 8 A3 F 8 BETA IEVTS F Define LMC material parameters using 8 parameters per card. Card Variable 1 P1 Type F 2 P2 F 3 P3 F 4 P4 F 5 P5 F 6 P6 F Define LMCA material parameters using 8 parameters per card. Card Variable 1 P1 Type F 2 P2 F 3 P3 F 4 P4 F 5 P5 F 6 P6 F 7 P7 F 7 P7 F 8 P8 F 8 P8 F VARIABLE DESCRIPTION MID RO MT LMC NHV Material identification. A unique number or label not exceeding 8 characters must be specified. Mass density. User material type (41 - 50 inclusive). A number between 41 and 50 has to be chosen. If MT < 0, subroutine rwumat in dyn21.f is called, where the material parameter reading can be modified. WARNING: If two or more materials in an input deck share the same MT value, those materials also share values of other variables on Cards 1 and 2 excluding MID and RO. Those shared values are taken from the first material where the common MT is encountered. Length of material constant array which is equal to the number of material constants to be input. Number of history variables to be stored, see Appendix A. When the model is to be used with an equation of state, NHV must be increased by 4 to allocate the storage required by the equation of state. VARIABLE IORTHO/ ISPOT DESCRIPTION EQ.1: if the material is orthotropic. EQ.2: if material is used with spot weld thinning. EQ.3: if material is orthotropic and used with spot weld thinning IBULK IG IVECT Address of bulk modulus in material constants array, see Appendix A. Address of shear modulus in material constants array, see Appendix A. Vectorization flag (on = 1). A vectorized user subroutine must be supplied. IFAIL Failure flag. EQ.0: No failure, EQ.1: Allows failure of shell and solid elements, LT.0: |IFAIL| is the address of NUMINT in the material constants array. NUMINT is defined as the number of failed integration points that will trigger element dele- tion. This option applies only to shell and solid elements (release 5 of version 971). ITHERM Temperature flag (on = 1). Compute element temperature. IHYPER Deformation gradient flag (on = 1 or –1, or 3). Compute defor- mation gradient, see Appendix A. IEOS Equation of state (on = 1). LMCA Length of additional material constant array. AOPT Material axes option : EQ.0.0: locally orthotropic with material axes determined by element nodes 1, 2, and 4, as with *DEFINE_COORDI- NATE_NODES, and then, for shells only, rotated about the shell element normal by an angle BETA. EQ.1.0: locally orthotropic with material axes determined by a point in space and the global location of the element center; this is the 𝑎-direction. This option is for solid VARIABLE DESCRIPTION elements only. EQ.2.0: globally orthotropic with material axes determined by vectors defined below, as with *DEFINE_COORDI- NATE_VECTOR. EQ.3.0: locally orthotropic material axes determined by rotating the material axes about the element normal by an angle, BETA, from a line in the plane of the element defined by the cross product of the vector 𝐯 with the element normal. EQ.4.0: locally orthotropic in cylindrical coordinate system with the material axes determined by a vector 𝐯, and an originating point, 𝐩, which define the centerline ax- is. This option is for solid elements only. LT.0.0: the absolute value of AOPT is a coordinate system ID number (CID on *DEFINE_COORDINATE_NODES, *DEFINE_COORDINATE_SYSTEM *DEFINE_ COORDINATE_VECTOR). Available in R3 version of 971 and later. or MACF Material axes change flag for brick elements for quick changes: EQ.1: No change, default, EQ.2: switch material axes 𝑎 and 𝑏, EQ.3: switch material axes 𝑎 and 𝑐, EQ.4: switch material axes 𝑏 and 𝑐. XP, YP, ZP Coordinates of point 𝐩 for AOPT = 1 and 4. A1, A2, A3 Components of vector 𝐚 for AOPT = 2. V1, V2, V3 Components of vector 𝐯 for AOPT = 3 and 4. D1, D2, D3 Components of vector 𝐝 for AOPT = 2. BETA IEVTS Material angle in degrees for AOPT = 0 (shells only) and AOPT = 3. BETA may be overridden on the element card, see *ELEMENT_SHELL_BETA and *ELEMENT_SOLID_ORTHO. Address of 𝐸𝑎 for orthotropic material in thick shell formulation 5 . P1 First material parameter. VARIABLE DESCRIPTION P2 P3 P4 ⋮ Second material parameter. Third material parameter. Fourth material parameter. ⋮ PLMC LMCth material parameter. Remarks: 1. Cohesive Elements. Material models for the cohesive element (solid element type 19) uses the first two material parameters to set flags in the element formula- tion. a) P1. The P1 field controls how the density is used to calculate the mass when determining the tractions at mid-surface (tractions are calculated on a surface midway between the surfaces defined by nodes 1-2-3-4 and 5-6- 7-8). If P1 is set to 1.0, then the density is per unit area of the midsurface instead of per unit volume. Note that the cohesive element formulation permits the element to have zero or negative volume. b) P2. The second parameter, P2, specifies the number of integration points (one to four) that are required to fail for the element to fail. If it is zero, the element will not fail regardless of IFAIL. The recommended value for P2 is 1. c) Other Parameters. The cohesive element only uses MID, RO, MT, LMC, NHV, IFAIL and IVECT in addition to the material parameters. d) Appendix R. See Appendix R for the specifics of the umat subroutine re- quirements for the cohesive element. 2. Material Constants. If IORTHO = 0, LMC must be ≤ 48. If IORTHO = 1, LMC must be ≤ 40. If more material constants are needed, LMCA may be used to create an additional material constant array. There is no limit on the size of LMCA. 3. Spot weld thinning. If the user-defined material is used for beam or brick element spot welds that are tied to shell elements, and SPOTHIN > 0 on *CON- TROL_CONTACT, then spot weld thinning will be done for those shells if IS- POT = 2. Otherwise, it will not be done. 4. Thick Shell Formulation 5. IEVTS is optional and is used only by thick shell formulation 5. It points to the position of 𝐸𝑎 in the material constants array. Following 𝐸𝑎, the next 5 material constants must be 𝐸𝑏, 𝐸𝑐, 𝜈𝑏𝑎, 𝜈𝑐𝑎, and 𝜈𝑐𝑏. This data enables thick shell formulation 5 to calculate an accurate thickness strain, otherwise the thickness strain will be based on the elastic constants pointed to by IBULK and IG. *MAT_BAMMAN This is Material Type 51. It allows the modeling of temperature and rate dependent plasticity with a fairly complex model that has many input parameters [Bamman 1989]. Card 1 1 Variable MID 2 RO Type A8 F Card 2 Variable 1 C1 Type F Card 3 Variable 1 C9 Type F Card 4 1 2 C2 F 2 F 2 Variable C17 C18 Type F F 3 E F 3 C3 F 3 4 PR F 4 C4 F 4 5 T F 5 C5 F 5 6 HC F 6 C6 F 6 7 8 7 C7 F 7 8 C8 F 8 C10 C11 C12 C13 C14 C15 C16 F F F F F 3 A1 F 4 A2 F 5 A4 F 6 A5 F 7 A6 F F 8 KAPPA F VARIABLE DESCRIPTION MID RO E Material identification. A unique number or label not exceeding 8 characters must be specified. Mass density. Young’s modulus (psi) VARIABLE DESCRIPTION PR T HC C1 C2 C3 C4 C5 C6 C7 C8 C9 C10 C11 C12 C13 C14 C15 C16 C17 C18 A1 A2 Poisson’s ratio Initial temperature (°R, degrees Rankine) Heat generation coefficient (°R⁄psi) Psi °R Psi °R 1/s °R 1/psi °R Psi °R 1/psi-s °R 1/psi °R psi °R 1/psi-s °R α1, initial value of internal state variable 1 α2, initial value of internal state variable 2. Note: α3 = -(α1 + α2 ) VARIABLE A3 A4 A5 DESCRIPTION α4, initial value of internal state variable 3 α5, initial value of internal state variable 4 α6, initial value of internal state variable 5 KAPPA κ, initial value of internal state variable 6 Unit Conversion Table Sec × psi × oR C1 C2 C3 C4 C5 C6 C7 C8 C9 C10 C11 C12 C13 C14 C15 C16 C17 C18 C0 = HC E T sec × MPa × oR × 1⁄145 — × 1⁄145 — — — × 145 — × 1⁄145 — × 145 — × 145 — × 1⁄145 — × 145 — × 145 × 1⁄145 — — sec × MPA × oK × 1⁄145 × 5⁄9 × 1⁄145 × 5⁄9 — × 5/9 × 145 × 5⁄9 × 1⁄145 × 5⁄9 × 145 × 5⁄9 × 145 × 5⁄9 × 1⁄145 × 5⁄9 × 145 × 5⁄9 × (145)(5⁄9) × 1⁄145 — × 5⁄9 *MAT_051 The kinematics associated with the model are discussed in references [Hill 1948, Bammann and Aifantis 1987, Bammann 1989]. The description below is taken nearly verbatim from Bammann [1989]. With the assumption of linear elasticity we can write, where the Cauchy stress σ is convected with the elastic spin 𝑾 𝑒 as, = 𝜆 tr(𝑫𝑒)𝟏 + 2𝜇𝑫𝑒 = 𝝈̇ − 𝑾 𝑒𝝈 + 𝝈𝑾 𝑒 This is equivalent to writing the constitutive model with respect to a set of directors whose direction is defined by the plastic deformation [Bammann and Aifantis 1987, Bammann and Johnson 1987]. Decomposing both the skew symmetric and symmetric parts of the velocity gradient into elastic and plastic parts we write for the elastic stretching 𝑫𝑒 and the elastic spin 𝑾 𝑒, 𝑫𝑒 = 𝑫 − 𝑫𝑝 − 𝑫𝑡ℎ, 𝑾 𝑒 = 𝑾 = 𝑾 𝑝. Within this structure it is now necessary to prescribe an equation for the plastic spin 𝑾 𝑝 in addition to the normally prescribed flow rule for 𝑫𝑝 and the stretching due to the thermal expansion 𝐷𝑡ℎ. As proposed, we assume a flow rule of the form, 𝑫𝑝 = 𝑓 (𝑇)sinh [ |𝜉 | − 𝜅 − 𝑌(𝑇) 𝑉(𝑇) ] 𝝃′ ∣𝜉′∣ . where T is the temperature, κ is the scalar hardening variable, and ξ′ is the difference between the deviatoric Cauchy stress σ′ and the tensor variable α′, 𝝃′ = 𝝈′ − 𝜶′ and f(T), Y(T), V(T) are scalar functions whose specific dependence upon the temperature is given below. Assuming isotropic thermal expansion and introducing the expansion coefficient Ȧ , the thermal stretching can be written, 𝑫𝑡ℎ = 𝐴̇𝑇̇𝟏 The evolution of the internal variables α and κ are prescribed in a hardening minus recovery format as, ⋅ = ℎ(𝑇)𝑫𝑝 − [𝑟𝑑(𝑇)|𝑫𝑝| + 𝑟𝑠(𝑇)]|𝜶|𝜶, = 𝐻(𝑇)𝑫𝑝 − [𝑅𝑑(𝑇)|𝑫𝑝| + 𝑅𝑠(𝑇)]𝜿2 where h and H are the hardening moduli, rs(T) and Rs(T) are scalar functions describing the diffusion controlled ‘static’ or ‘thermal’ recovery, and rd(T) and Rd(T) are the functions describing dynamic recovery. If we assume that Wp = 0, we recover the Jaumann stress rate which results in the prediction of an oscillatory shear stress response in simple shear when coupled with a Prager kinematic hardening assumption [Johnson and Bammann 1984]. Alternatively we can choose, 𝑾 𝑝 = 𝑹𝑇𝑼̇ 𝑼 −1𝑹, which recovers the Green-Naghdi rate of Cauchy stress and has been shown to be equivalent to Mandel’s isoclinic state [Bammann and Aifantis 1987]. The model employing this rate allows a reasonable prediction of directional softening for some materials, but in general under-predicts the softening and does not accurately predict the axial stresses which occur in the torsion of the thin walled tube. The final equation necessary to complete our description of high strain rate deformation is one which allows us to compute the temperature change during the deformation. In the absence of a coupled thermo-mechanical finite element code we assume adiabatic temperature change and follow the empirical assumption that 90 -95% of the plastic work is dissipated as heat. Hence, 𝑇̇ = . 9 𝜌𝐶𝑣 (𝝈 ⋅ 𝑫𝑝), where ρ is the density of the material and Cv the specific heat. In terms of the input parameters the functions defined above become: V(T) = C1 exp(-C2/T) h(T) = C9 exp(C10/T) Y(T) = C3 exp(C4/T) rs(T) = C11exp(-C12/T) f(T) = C5 exp(-C6/T) RD(T) = C13exp(-C14/T) rd(T) = C7 exp(-C8/T) H(T) = C15exp(C16/T) RS(T) = C17exp(-C18/T) and the heat generation coefficient is 𝐻𝐶 = 0.9 𝜌𝐶𝑣 . *MAT_052 This is Material Type 52. This is an extension of model 51 which includes the modeling of damage. See Bamman et al. [1990]. Card 1 1 Variable MID 2 RO Type A8 F Card 2 Variable 1 C1 Type F Card 3 Variable 1 C9 Type F Card 4 1 2 C2 F 2 F 2 Variable C17 C18 Type F F Card 5 Variable Type 1 N F 2 D0 F 3 E F 3 C3 F 3 4 PR F 4 C4 F 4 5 T F 5 C5 F 5 6 HC F 6 C6 F 6 7 8 7 C7 F 7 8 C8 F 8 F F F F F F 4 A2 F 4 5 A3 F 5 6 A4 F 6 7 A5 F 7 8 A6 F 8 3 A1 F 3 FS F C10 C11 C12 C13 C14 C15 C16 MID *MAT_BAMMAN_DAMAGE DESCRIPTION Material identification. A unique number or label not exceeding 8 characters must be specified. RO E PR T HC C1 C2 C3 C4 C5 C6 C7 C8 C9 C10 C11 C12 C13 C14 C15 C16 Mass density Young’s modulus (psi) Poisson’s ratio Initial temperature (°R, degrees Rankine) Heat generation coefficient (°R⁄psi) Psi °R Psi °R 1/s °R 1/psi °R Psi oR 1/psi-s °R 1/psi °R psi °R VARIABLE DESCRIPTION C17 C18 A1 A2 A3 A4 A5 A6 N D0 FS 1/psi-s °R 1, initial value of internal state variable 1 2, initial value of internal state variable 2 3, initial value of internal state variable 3 4, initial value of internal state variable 4 α5, initial value of internal state variable 5 α6, initial value of internal state variable 6 Exponent in damage evolution Initial damage (porosity) Failure strain for erosion. Remarks: The evolution of the damage parameter, φ is defined by Bammann et al. [1990] in which 𝜙̇ = 𝛽 [ (1 − 𝜙)𝑁 − (1 − 𝜙)] ∣𝑫𝑝∣ 𝛽 = sinh [ 2(2𝑁 − 1)𝑝 (2𝑁 − 1)𝜎̅̅̅̅̅ ] where p is the pressure and 𝜎̅̅̅̅̅ is the effective stress. *MAT_CLOSED_CELL_FOAM This is Material Type 53. This allows the modeling of low density, closed cell polyurethane foam. It is for simulating impact limiters in automotive applications. The effect of the confined air pressure is included with the air being treated as an ideal gas. The general behavior is isotropic with uncoupled components of the stress tensor. 3 E F 3 4 A F 4 5 B F 5 6 C F 6 7 P0 F 7 8 PHI F 8 Card 1 1 Variable MID Type A8 Card 2 1 2 RO F 2 Variable GAMA0 LCID Type F I VARIABLE MID DESCRIPTION Material identification. A unique number or label not exceeding 8 characters must be specified. RO Mass density E A B C P0 PHI Young’s modulus a, factor for yield stress definition, see notes below. b, factor for yield stress definition, see notes below. c, factor for yield stress definition, see notes below. Initial foam pressure, P0 Ratio of foam to polymer density, φ GAMA0 Initial volumetric strain, γ0. The default is zero. DESCRIPTION Optional load curve defining the von Mises yield stress versus −𝛾. If the load curve ID is given, the yield stress is taken from the curve and the constants a, b, and c are not needed. The load curve is defined in the positive quadrant, i.e., positive values of 𝛾 are defined as negative values on the abscissa. VARIABLE LCID Remarks: A rigid, low density, closed cell, polyurethane foam model developed at Sandia Laboratories [Neilsen, Morgan and Krieg 1987] has been recently implemented for modeling impact limiters in automotive applications. A number of such foams were tested at Sandia and reasonable fits to the experimental data were obtained. In some respects this model is similar to the crushable honeycomb model type 26 in that the components of the stress tensor are uncoupled until full volumetric compaction is achieved. However, unlike the honeycomb model this material possesses no directionality but includes the effects of confined air pressure in its overall response characteristics. 𝜎𝑖𝑗 = 𝜎𝑖𝑗 sk − 𝛿𝑖𝑗𝜎 air where 𝜎𝑖𝑗 𝑠𝑘 is the skeletal stress and 𝜎 𝑎𝑖𝑟 is the air pressure computed from the equation: 𝜎 air = − 𝑝0𝛾 1 + 𝛾 − 𝜙 where p0 is the initial foam pressure, usually taken as the atmospheric pressure, and γ defines the volumetric strain 𝛾 = 𝑉 − 1 + 𝛾0 where V is the relative volume, defined as the ratio of the current volume to the initial volume, and γ0 is the initial volumetric strain, which is typically zero. The yield condition is applied to the principal skeletal stresses, which are updated independently of the air pressure. We first obtain the skeletal stresses: and compute the trial stress, σskt 𝜎𝑖𝑗 sk = 𝜎𝑖𝑗 + 𝜎𝑖𝑗𝜎 air skt = 𝜎𝑖𝑗 𝜎𝑖𝑗 sk + 𝐸 𝜀̇𝑖𝑗 Δ𝑡 where E is Young’s modulus. Since Poisson’s ratio is zero, the update of each stress component is uncoupled and 2G = E where G is the shear modulus. The yield condition is applied to the principal skeletal stresses such that, if the magnitude of a principal trial stress component, 𝜎𝑖 𝑠𝑘𝑡, exceeds the yield stress, σ y, then sk = min(𝜎𝑦, ∣𝜎𝑖 𝜎𝑖 skt∣) skt skt∣ 𝜎𝑖 ∣𝜎𝑖 The yield stress is defined by 𝜎𝑦 = 𝑎 + 𝑏(1 + 𝑐𝛾) where a, b, and c are user defined input constants and γ is the volumetric strain as defined above. After scaling the principal stresses they are transformed back into the global system and the final stress state is computed 𝜎𝑖𝑗 = 𝜎𝑖𝑗 sk − 𝛿𝑖𝑗𝜎 air. *MAT_ENHANCED_COMPOSITE_DAMAGE These are Material Types 54 - 55 which are enhanced versions of the composite model material type 22. Arbitrary orthotropic materials, e.g., unidirectional layers in composite shell structures can be defined. Optionally, various types of failure can be specified following either the suggestions of [Chang and Chang 1987b] or [Tsai and Wu 1971]. In addition special measures are taken for failure under compression. See [Matzenmiller and Schweizerhof 1991]. By using the user defined integration rule, see *INTEGRATION_SHELL, the constitutive constants can vary through the shell thickness. For all shells, except the DKT formulation, laminated shell theory can be activated to properly model the transverse shear deformation. Lamination theory is applied to correct for the assumption of a uniform constant shear strain through the thickness of the shell. For sandwich shells where the outer layers are much stiffer than the inner layers, the response will tend to be too stiff unless lamination theory is used. To turn on lamination theory see *CONTROL_SHELL. A damage model for transverse shear strain to model interlaminar shear failure is available. The definition of minimum stress limits is available for thin/thick shells and solids. Card 1 1 Variable MID Type A8 Card 2 1 2 RO F 2 3 EA F 3 4 EB F 4 5 EC F 5 Variable GAB GBC GCA (KF) AOPT 2WAY Type F Card 3 1 F 2 F 3 Variable Type F F 4 A1 F 5 A2 F 6 7 8 PRBA PRCA PRCB F 6 F 6 F 7 TI F 7 F 8 8 A3 MANGLE F Card 4 Variable 1 V1 Type F Card 5 1 2 V2 F 2 3 V3 F 3 4 D1 F 4 5 D2 F 5 6 7 8 D3 DFAILM DFAILS F 6 F 7 F 8 Variable TFAIL ALPH SOFT FBRT YCFAC DFAILT DFAILC EFS Type F F F F F Card 6 Variable 1 XC Type F 2 XT F 3 YC F 4 YT F 5 SC F F 6 F 7 F 8 CRIT BETA F F Optional Card 7 (only for CRIT = 54) Card 7 1 2 3 4 5 6 7 8 Variable PFL EPSF EPSR TSMD SOFT2 Type F F F F F Optional Card 8 (only for CRIT = 54) Card 8 1 2 3 4 5 6 7 8 Variable SLIMT1 SLIMC1 SLIMT2 SLIMC2 SLIMS NCYRED SOFTG Type F F F F F F Optional Card 9 (only for CRIT = 54) Card 9 1 2 3 4 5 Variable LCXC LCXT LCYC LCYT LCSC Type I I I I I 7 8 6 DT F VARIABLE DESCRIPTION MID RO EA EB EC PRBA PRCA PRCB GAB GBC GCA (KF) AOPT Material identification. A unique number or label not exceeding 8 characters must be specified. Mass density 𝐸𝑎, Young’s modulus - longitudinal direction 𝐸𝑏, Young’s modulus - transverse direction 𝐸𝑐, Young’s modulus - normal direction 𝜈𝑏𝑎, Poisson’s ratio 𝑏𝑎 𝜈𝑐𝑎, Poisson’s ratio 𝑐𝑎 𝜈𝑐𝑏, Poisson’s ratio 𝑐𝑏 𝐺𝑎𝑏, shear modulus 𝑎𝑏 𝐺𝑏𝑐, shear modulus 𝑏𝑐 𝐺𝑐𝑎, shear modulus 𝑐𝑎 Bulk modulus of failed material (not used) Material axes option : EQ.0.0: locally orthotropic with material axes determined by element nodes 1, 2, and 4, as with *DEFINE_COORDI- NATE_NODES, and then, for shells only, rotated about the shell element normal by an angle MANGLE. EQ.2.0: globally orthotropic with material axes determined by vectors defined below, as with *DEFINE_COORDI- NATE_VECTOR. EQ.3.0: locally orthotropic material axes determined by VARIABLE DESCRIPTION rotating the material axes about the element normal by an angle (MANGLE) from a line in the plane of the el- ement defined by the cross product of the vector v with the element normal. EQ.4.0: locally orthotropic in cylindrical coordinate system with the material axes determined by a vector 𝐯, and an originating point, 𝐩, which define the centerline axis. This option is for solid elements only. LT.0.0: the absolute value of AOPT is a coordinate system ID number (CID on *DEFINE_COORDINATE_NODES, *DEFINE_COORDINATE_SYSTEM or *DEFINE_CO- ORDINATE_VECTOR). Available in R3 version of 971 and later. 2WAY Flag to turn on 2-way fiber action. EQ.0.0: Standard unidirectional behavior. EQ.1.0: 2-way fiber behavior. The meaning of the fields DFAILT, DFAILC, YC, YT, SLIMT2 and SLIMC2 are altered if this flag is set. This option is only available for MAT 54 using thin shells. TI Flag to turn on transversal isotropic behavior for MAT_054 solid elements. EQ.0.0: Standard unidirectional behavior. EQ.1.0: transversal isotropic behavior . A1, A2, A3 Define components of vector 𝐚 for AOPT = 2. V1, V2, V3 Define components of vector 𝐯 for AOPT = 3. D1, D2, D3 Define components of vector 𝐝 for AOPT = 2. MANGLE Material angle in degrees for AOPT = 0 (shells only) and AOPT = 3. MANGLE may be overridden on the element card, see *ELEMENT_SHELL_BETA and *ELEMENT_SOLID_ORTHO. VARIABLE DFAILM DESCRIPTION Maximum strain for matrix straining in tension or compression (active only for MAT_054 and only if DFAILT > 0). The layer in the element is completely removed after the maximum strain in the matrix direction is reached. The input value is always positive. DFAILS Maximum tensorial shear strain (active only for MAT_054 and only if DFAILT > 0). The layer in the element is completely removed after the maximum shear strain is reached. The input value is always positive. TFAIL Time step size criteria for element deletion: tfail ≤ 0: no element deletion by time step size. The crashfront algorithm only works if tfail is set to a value above zero. 0 < tfail ≤ 0.1: element is deleted when its time step is smaller than the given value, tfail > 0.1: element is deleted when the quotient of the actual time step and the original time step drops below the given value. ALPH SOFT Shear stress parameter for the nonlinear term, see Material 22. Softening reduction factor for material strength in crashfront elements (default = 1.0). TFAIL must be greater than zero to activate this option. FBRT Softening for fiber tensile strength: EQ.0.0: tensile strength = XT GT.0.0: tensile strength = XT, reduced to XT × FBRT after failure has occurred in compressive matrix mode. YCFAC Reduction factor for compressive fiber strength after matrix compressive failure (MAT_054 only). The compressive strength in the fiber direction after compressive matrix failure is reduced to: 𝑋𝑐 = YCFAC × 𝑌𝑐, (default: YCFAC = 2.0) VARIABLE DFAILT DESCRIPTION Maximum strain for fiber tension (MAT_054 only). (Maximum 1 = 100% strain). The layer in the element is completely removed after the maximum tensile strain in the fiber direction is reached. If a nonzero value is given for DFAILT, a nonzero, negative value must also be provided for DFAILC. If the 2-way fiber flag is set then DFAILT is the fiber tensile failure strain in the 𝑎 and 𝑏 directions. DFAILC EFS XC XT YC for fiber compression (MAT_054 only). Maximum strain (Maximum -1 = 100% compression). The layer in the element is completely removed after the maximum compressive strain in the fiber direction is reached. The input value should be negative and is required if DFAILT > 0. If the 2-way fiber flag is set then DFAILC is the fiber compressive failure strain in the 𝑎 and 𝑏 directions. Effective failure strain (MAT_054 only). Longitudinal compressive strength (absolute value is used). GE.0.0: Poisson effect (PRBA) after failure is active. LT.0.0: Poisson effect after failure is not active, i.e. PRBA = 0. Longitudinal tensile strength, see below. Transverse compressive strength, 𝑏-axis (positive value), see below. If the 2-way fiber flag is set then YC is the fiber compressive failure stress in the 𝑏 direction. YT Transverse tensile strength, 𝑏-axis, see below. If the 2-way fiber flag is set then YT is the fiber tensile failure stress in the 𝑏 direction. SC Shear strength, ab plane, see below. VARIABLE DESCRIPTION CRIT Failure criterion (material number): BETA PFL EPSF EPSR TSMD SOFT2 SLIMT1 SLIMC1 SLIMT2 EQ.54.0: Chang criterion for matrix failure (as Material 22) (default), EQ.55.0: Tsai-Wu criterion for matrix failure. Weighting factor for shear term in tensile fiber mode (MAT_054 only). (0.0 ≤ BETA ≤ 1.0) Percentage of layers which must fail until crashfront is initiated. E.g. |PFL| = 80.0, then 80% of layers must fail until strengths are reduced in neighboring elements. Default: all layers must fail. A single layer fails if 1 in-plane IP fails (PFL > 0) or if 4 in-plane IPs fail (PFL < 0). (MAT_054 only, thin and thick shells). Damage initiation transverse shear strain. (MAT_054 only). Final rupture transverse shear strain. (MAT_054 only). Transverse shear maximum damage, default = 0.90. (MAT_054 only,). Optional “orthogonal” softening reduction factor for material strength in crashfront elements (default = 1.0). See remarks (MAT_054 only, thin and thick shells). Factor to determine the minimum stress limit after stress maximum (fiber tension). Similar to *MAT_058 (MAT_054 only). Factor to determine the minimum stress limit after stress maximum (fiber compression). Similar to *MAT_058 (MAT_054 only). Factor to determine the minimum stress limit after stress maximum (matrix tension). Similar to *MAT_058 (MAT_054 only). If the 2-way fiber flag is set then SLIMT2 is the factor to determine the minimum stress limit after tensile failure stress is reached in the 𝑏 fiber direction. VARIABLE SLIMC2 SLIMS NCYRED SOFTG LCXC LCXT LCYC LCYT LCSC DESCRIPTION Factor to determine the minimum stress limit after stress maximum (matrix compression). Similar to *MAT_058 (MAT_054 only). If the 2-way fiber flag is set then SLIMC2 is the factor to determine the minimum stress limit after compressive failure stress is reached in the 𝑏 fiber direction. Factor to determine the minimum stress limit after stress maximum (shear). Similar to *MAT_058 (MAT_054 only). Number of cycles for stress reduction from maximum to minimum (MAT_054 only). Softening reduction factor for transverse shear moduli GBC and GCA in crashfront elements (default = 1.0) (MAT_054 only, thin and thick shells). Load curve ID for XC vs. strain rate (XC is ignored with that option) Load curve ID for XT vs. strain rate (XT is ignored with that option) Load curve ID for YC vs. strain rate (YC is ignored with that option) Load curve ID for YT vs. strain rate (YT is ignored with that option) Load curve ID for SC vs. strain rate (SC is ignored with that option) DT Strain rate averaging option. EQ.0.0: Strain rate is evaluated using a running average. LT.0.0: Strain rate is evaluated using average of last 11 time steps. GT.0.0: Strain rate is averaged over the last DT time units. Material Formulation: The Chang/Chang (MAT_54) criteria is given as follows: for the tensile fiber mode, 𝜎𝑎𝑎 > 0 ⇒ 𝑒𝑓 2 = ( ) 𝜎𝑎𝑎 𝑋𝑡 + 𝛽 ( 𝜎𝑎𝑏 𝑆𝑐 ) − 1, 2 ≥ 0 ⇒ failed 𝑒𝑓 2 < 0 ⇒ elastic 𝑒𝑓 𝐸𝑎 = 𝐸𝑏 = 𝐺𝑎𝑏 = 𝜈𝑏𝑎 = 𝜈𝑎𝑏 = 0 for the compressive fiber mode, 𝜎𝑎𝑎 < 0 ⇒ 𝑒𝑐 2 = ( − 1, ) 𝜎𝑎𝑎 𝑋𝑐 2 ≥ 0 ⇒ failed 𝑒𝑐 2 < 0 ⇒ elastic 𝑒𝑐 𝐸𝑎 = 𝜈𝑏𝑎 = 𝜈𝑎𝑏 = 0 for the tensile matrix mode, 𝜎𝑏𝑏 > 0 ⇒ 𝑒𝑚 2 = ( 𝜎𝑏𝑏 𝑌𝑡 ) + ( 𝜎𝑎𝑏 𝑆𝑐 ) − 1, 2 ≥ 0 ⇒ failed 𝑒𝑚 2 < 0 ⇒ elastic 𝑒𝑚 𝐸𝑏 = 𝜈𝑏𝑎 = 0 ⇒ 𝐺𝑎𝑏 = 0, and for the compressive matrix mode, 𝜎𝑏𝑏 < 0 ⇒ 𝑒𝑑 2 = ( 𝜎𝑏𝑏 2𝑆𝑐 ) + ) 𝑌𝑐 2𝑆𝑐 ⎢⎡( ⎣ − 1 ⎥⎤ 𝜎𝑏𝑏 𝑌𝑐 ⎦ + ( ) 𝜎𝑎𝑏 𝑆𝑐 − 1, 2 ≥ 0 ⇒ failed 𝑒𝑑 2 < 0 ⇒ elastic 𝑒𝑑 𝐸𝑏 = 𝜈𝑏𝑎 = 𝜈𝑎𝑏 = 0 ⇒ 𝐺𝑎𝑏 = 0 𝑋𝑐 = 2𝑌𝑐, for 50% fiber volume If the 2-way fiber flag is set then the failure criteria for tensile and compressive fiber failure in the local X direction are unchanged. For the local 𝑦-direction, the same failure criteria as for the 𝑥-direction fibers are used. Tension, 𝑦-direction, 𝜎𝑏𝑏 > 0 ⇒ 𝑒𝑓 2 = ( ) 𝜎𝑏𝑏 𝑌𝑡 + 𝛽 ( 𝜎𝑎𝑏 𝑆𝑐 ) − 1, 2 ≥ 0 ⇒ failed 𝑒𝑓 2 < 0 ⇒ elastic 𝑒𝑓 Compressive 𝑦-direction, 𝜎𝑏𝑏 < 0 ⇒ 𝑒𝑐 2 = ( 𝜎𝑏𝑏 𝑌𝑐 ) − 1, 2 ≥ 0 ⇒ failed 𝑒𝑐 2 < 0 ⇒ elastic 𝑒𝑐 Matrix failure criterion, 2 = ( 𝑒𝑓 ) 𝜎𝑎𝑏 𝑆𝑐 − 1 In the Tsai-Wu (MAT_055) criteria the tensile and compressive fiber modes are treated as in the Chang-Chang criteria. The failure criterion for the tensile and compressive matrix mode is given as: 2 = 𝑒md 𝜎𝑏𝑏 𝑌𝑐𝑌𝑡 + ( ) 𝜎𝑎𝑏 𝑆𝑐 + (𝑌𝑐 − 𝑌𝑡) 𝜎𝑏𝑏 𝑌𝑐𝑌𝑡 − 1, 2 ≥ 0 ⇒ failed 𝑒𝑚𝑑 2 < 0 ⇒ elastic 𝑒𝑚𝑑 For β = 1 we get the original criterion of Hashin [1980] in the tensile fiber mode. For β = 0 we get the maximum stress criterion which is found to compare better to experiments. In MAT_054, failure can occur in any of four different ways: 1. 2. 3. 4. If DFAILT is zero, failure occurs if the Chang-Chang failure criterion is satisfied in the tensile fiber mode. If DFAILT is greater than zero, failure occurs if: - - - the fiber strain is greater than DFAILT or less than DFAILC if absolute value of matrix strain is greater than DFAILM if absolute value of tensorial shear strain is greater than DFAILS If EFS is greater than zero, failure occurs if the effective strain is greater than EFS. If TFAIL is greater than zero, failure occurs according to the element timestep as described in the definition of TFAIL above. When failure has occurred in all the composite layers (through-thickness integration points), the element is deleted. Elements which share nodes with the deleted element become “crashfront” elements and can have their strengths reduced by using the SOFT parameter with TFAIL greater than zero. An earlier initiation of crashfront elements is possible by using parameter PFL. Reduction by SOFT2 (orthogonal ) Reduction by 0.5(SOFT+SOFT2) Reduction By SOFT (parallel) Figure M54-1. Direction dependent softening An optional direction dependent strength reduction can be invoked by setting 0 < SOFT2 < 1. Then, SOFT equals a strength reduction factor for fiber parallel failure and SOFT2 equals a strength reduction factor for fiber orthogonal failure. Linear interpolation is used for angles in between. See Figure M54-1. Information about the status in each layer (integration point) and element can be plotted using additional integration point variables. The number of additional integration point variables for shells written to the LS-DYNA database is input by the *DATABASE_EXTENT_BINARY definition as variable NEIPS. For Models 54 and 55 these additional variables are tabulated below (i = shell integration point): History Variable 1 ef(i) Description tensile fiber mode Value LS-PrePost History Variable 2 ec(i) compressive fiber mode 3 em(i) tensile matrix mode 1 – elastic 4 ed(i) compressive mode 5 efail max[ef(ip)] matrix 0 – failed 6 dam damage parameter −1 – element intact 10−8 – element crashfront +1 – element failed in 1 2 3 4 5 6 These variables can be plotted in LS-PrePost element history variables 1 to 6. The following components, defined by the sum of failure indicators over all through- thickness integration points, are stored as element component 7 instead of the effective plastic strain. Description Integration point nip nip ∑ 𝑒𝑓 (𝑖) 𝑖=1 nip nip ∑ 𝑒𝑐(𝑖) 𝑖=1 nip nip ∑ 𝑒𝑚(𝑖) 𝑖=1 1 2 3 In an optional damage model for transverse shear strain, out-of-plane stiffness (GBC and GCA) can get linearly decreased to model interlaminar shear failure. Damage starts when effective transverse shear strain eff = √𝜀𝑦𝑧 𝜀56 2 2 + 𝜀𝑧𝑥 reaches EPSF. Final rupture occurs when effective transverse shear strain reaches EPSR. A maximum damage of TSMD (0.0 < TSMD < 0.99) cannot be exceeded. See Figure M54-2. transverse shear stiffness transverse shear stiffness GBC, GBC, GCA GCA D=0 D = 0 D=TSMD D = TSMD EPSF EPSF EPSR EPSR transverse shear strain transverse shear strain Figure M54-3. Linear Damage for transverse shear behavior Figure M54-2. Linear Damage for transverse shear behavior Additional Remarks: 1. TI-Flag (Transversal isotropic behavior for *MAT_054 solid elements). The behavior in the b-c-plane is assumed to be isotropic, thus the elastic constants EC, PRCA and GCA are ignored and set according to the given values EA, EB, PRAB, GAB. Damage in transverse shear (EPSF, EPSR, TSMD, SOFTG) is ignored. The failure criterion is evaluated by replacing 𝜎bb and 𝜎ab with the corresponding stresses 𝜎11 and 𝜎a1 in a principal stress frame rotated around the local a-axis. The principal axes 1 and 2 in the b-c plane are chosen such that |𝜎11| ≥ |𝜎22| is fulfilled. *MAT_LOW_DENSITY_FOAM This is Material Type 57 for modeling highly compressible low density foams. Its main applications are for seat cushions and padding on the Side Impact Dummies (SID). Optionally, a tension cut-off failure can be defined. A table can be defined if thermal effects are considered in the nominal stress versus strain behavior. Also, see the notes below. Card 1 1 Variable MID 2 RO Type A8 F 3 E F 4 LCID F Default Remarks 5 TC F 1020 Card 2 1 2 3 4 5 6 HU F 1. 3 6 7 8 BETA DAMP F F 0.05 8 1 7 Variable SHAPE FAIL BVFLAG ED BETA1 KCON REF Type F F F F F F F Default 1.0 0.0 0.0 0.0 0.0 0.0 0.0 Remarks 3 2 5 5 6 VARIABLE DESCRIPTION MID RO E Material identification. A unique number or label not exceeding 8 characters must be specified. Mass density Young’s modulus used in tension. For implicit problems E is set to the initial slope of load curve LCID. VARIABLE LCID TC HU BETA DAMP DESCRIPTION Load curve or table ID, see *DEFINE_CURVE, for the nominal stress versus strain curve definition. If a table is used, a family of curves is defined each corresponding to a discrete temperature, see *DEFINE_TABLE. Cut-off for the nominal tensile stress τi Hysteretic unloading factor between 0 and 1 (default = 1, i.e., no energy dissipation), see also Figure M57-1. β, decay constant to model creep in unloading Viscous coefficient (.05 < recommended value <.50) to model damping effects. LT.0.0: |DAMP| is the load curve ID, which defines the damping constant as a function of the maximum strain in compression defined as: 𝜀max = max(1 − 𝜆1, 1 − 𝜆2, 1. −𝜆3). In tension, the damping constant is set to the value corre- sponding to the strain at 0. The abscissa should be defined from 0 to 1. SHAPE Shape factor for unloading. Active for nonzero values of the hysteretic unloading factor. Values less than one reduces the energy dissipation and greater than one increases dissipation, see also Figure M57-1. FAIL Failure option after cutoff stress is reached: EQ.0.0: tensile stress remains at cut-off value, EQ.1.0: tensile stress is reset to zero. BVFLAG Bulk viscosity activation flag, see remark below: EQ.0.0: no bulk viscosity (recommended), EQ.1.0: bulk viscosity active. ED Optional Young's relaxation modulus, 𝐸𝑑, for rate effects. See Remark 5. BETA1 Optional decay constant, 𝛽1. Typical unloading curves determined by the hysteretic unloading factor. With the shape factor equal to unity. Typical unloading for a large shape factor, e.g. 5.0-8.0, and a small hystereticfactor, e.g., 0.010. Unloading curves Strain Strain Figure M57-1. Behavior of the low density urethane foam model VARIABLE KCON DESCRIPTION Stiffness coefficient for contact interface stiffness. If undefined the maximum slope in stress vs. strain curve is used. When the maximum slope is taken for the contact, the time step size for this material is reduced for stability. In some cases Δt may be significantly smaller, and defining a reasonable stiffness is recommended. REF Use reference geometry to initialize the stress tensor. The reference geometry is defined by the keyword:*INITIAL_FOAM_- REFERENCE_GEOMETRY . EQ.0.0: off, EQ.1.0: on. Material Formulation: The compressive behavior is illustrated in Figure M57-1 where hysteresis on unloading is shown. This behavior under uniaxial loading is assumed not to significantly couple in the transverse directions. In tension the material behaves in a linear fashion until tearing occurs. Although our implementation may be somewhat unusual, it was motivated by Storakers [1986]. The model uses tabulated input data for the loading curve where the nominal stresses are defined as a function of the elongations, 𝜀𝑖, which are defined in terms of the principal stretches, 𝜆𝑖, as: 𝜀𝑖 = 𝜆𝑖 − 1 The principal stretches are stored as extra history variables 16, 17, and 18 if ED = 0 and as extra history variables 28, 29, and 30 if ED > 0. The stretch ratios are found by solving for the eigenvalues of the left stretch tensor, 𝑉𝑖𝑗, which is obtained via a polar decomposition of the deformation gradient matrix, 𝐹𝑖𝑗. Recall that, 𝐹𝑖𝑗 = 𝑅𝑖𝑘𝑈𝑘𝑗 = 𝑉𝑖𝑘𝑅𝑘𝑗 The update of Vij follows the numerically stable approach of Taylor and Flanagan [1989]. After solving for the principal stretches, we compute the elongations and, if the elongations are compressive, the corresponding values of the nominal stresses, 𝜏𝑖 are interpolated. If the elongations are tensile, the nominal stresses are given by and the Cauchy stresses in the principal system become 𝜏𝑖 = 𝐸𝜀𝑖 𝜎𝑖 = 𝜏𝑖 𝜆𝑗𝜆𝑘 The stresses can now be transformed back into the global system for the nodal force calculations. Remarks: 1. When hysteretic unloading is used the reloading will follow the unloading curve if the decay constant, β, is set to zero. If β is nonzero the decay to the original loading curve is governed by the expression: 1 − 𝑒−𝛽𝑡 2. The bulk viscosity, which generates a rate dependent pressure, may cause an unexpected volumetric response and, consequently, it is optional with this model. 3. The hysteretic unloading factor results in the unloading curve to lie beneath the loading curve as shown in Figure M57-1 This unloading provides energy dissi- pation which is reasonable in certain kinds of foam. 4. Note that since this material has no effective plastic strain, the internal energy per initial volume is written into the output databases. 5. Rate effects are accounted for through linear viscoelasticity by a convolution integral of the form 𝜎𝑖𝑗 𝑟 = ∫ 𝑔𝑖𝑗𝑘𝑙 (𝑡 − 𝜏) ∂𝜀𝑘𝑙 ∂𝜏 𝑑𝜏 where 𝑔𝑖𝑗𝑘𝑙(𝑡 − 𝜏) is the relaxation function. The stress tensor, 𝜎𝑖𝑗 stresses determined from the foam, 𝜎𝑖𝑗 taken as the summation of the two contributions: 𝑟 , augments the 𝑓 ; consequently, the final stress, 𝜎𝑖𝑗, is 𝜎𝑖𝑗 = 𝜎𝑖𝑗 𝑓 + 𝜎𝑖𝑗 𝑟 . Since we wish to include only simple rate effects, the relaxation function is represented by one term from the Prony series: given by, 𝑔(𝑡) = 𝛼0 + ∑ 𝛼𝑚 𝑚=1 𝑒−𝛽 𝑡 𝑔(𝑡) = 𝐸𝑑𝑒−𝛽1 𝑡 This model is effectively a Maxwell fluid which consists of a damper and spring in series. We characterize this in the input by a Young's modulus, 𝐸𝑑, and de- cay constant, 𝛽1. The formulation is performed in the local system of principal stretches where only the principal values of stress are computed and triaxial coupling is avoided. Consequently, the one-dimensional nature of this foam material is unaffected by this addition of rate effects. The addition of rate ef- fects necessitates twelve additional history variables per integration point. The cost and memory overhead of this model comes primarily from the need to “remember” the local system of principal stretches. 6. The time step size is based on the current density and the maximum of the instantaneous loading slope, 𝐸, and KCON. If KCON is undefined the maxi- mum slope in the loading curve is used instead. *MAT_LAMINATED_COMPOSITE_FABRIC This is Material Type 58. Depending on the type of failure surface, this model may be used to model composite materials with unidirectional layers, complete laminates, and woven fabrics. This model is implemented for shell and thick shell elements (ELFORM = 1 and 2). Card 1 1 Variable MID Type A8 Card 2 1 2 RO F 2 3 EA F 3 4 EB F 4 5 6 7 8 (EC) PRBA TAU1 GAMMA1 F 5 F 6 F 7 F 8 Variable GAB GBC GCA SLIMT1 SLIMC1 SLIMT2 SLIMC2 SLIMS Type F Card 3 1 F 2 F 3 F 4 Variable AOPT TSIZE ERODS SOFT Type F F F F Card 4 Variable 1 XP Type F Card 5 Variable 1 V1 Type F LS-DYNA R10.0 2 YP F 2 V2 F 3 ZP F 3 V3 F 4 A1 F 4 D1 F F 5 FS F 5 A2 F 5 D2 F F 6 F 7 F 8 EPSF EPSR TSMD F 6 A3 F 6 D3 F F 7 F 8 PRCA PRCB F 8 F 7 BETA Card 6 1 2 3 4 5 6 7 8 Variable E11C E11T E22C E22T GMS Type F F F F F Card 7 Variable 1 XC Type F 2 XT F 3 YC F 4 YT F 5 SC F 6 7 8 First Optional Strain Rate Dependence Card. Card 8 1 2 3 4 5 6 7 8 Variable LCXC LCXT LCYC LCYT LCSC LCTAU LCGAM DT Type I I I I I I I F Second Optional Strain Rate Dependence Card. Card 9 1 2 3 4 5 6 7 8 Variable LCE11C LCE11T LCE22C LCE22T LCGMS LCEFS Type I I I I I I VARIABLE MID DESCRIPTION Material identification. A unique number or label not exceeding 8 characters must be specified. RO Mass density VARIABLE EA DESCRIPTION GT.0.0: 𝐸𝑎, Young’s modulus - longitudinal direction LT.0.0: Load curve ID or Table ID = (-EA) Load Curve. When (-EA) is equal to a Load curve ID, it is taken as defining the uniaxial elastic stress vs. strain behavior in longitudinal direction. Tabular Data. When (-EA) is equal to a Table ID, it defines for each strain rate value a Load curve ID giv- ing the uniaxial elastic stress vs. strain behavior in longitudinal direction. Logarithmically Defined Tables. If the first uniaxial elastic stress vs. strain curve in the table corresponds to a negative strain rate, LS-DYNA assumes that the natural logarithm of the strain rate value is used for all stress-strain curves. EB GT.0.0: 𝐸𝑏, Young’s modulus - transverse direction LT.0.0: Load curve ID or Table ID = (-EB) Load Curve. When (-EB) is equal to a Load curve ID, it is taken as defining the uniaxial elastic stress vs. strain behavior in transverse direction. Tabular Data. When (-EB) is equal to a Table ID, it defines for each strain rate value a Load curve ID giv- ing the uniaxial elastic stress vs. strain behavior in transverse direction. Logarithmically Defined Tables. If the first uniaxial elastic stress vs. strain curve in the table corresponds to a negative strain rate, LS-DYNA assumes that the natural logarithm of the strain rate value is used for all stress-strain curves. (EC) PRBA PRCA PRCB Ec, Young’s modulus - normal direction (not used) 𝜈𝑏𝑎, Poisson’s ratio ba 𝜈𝑐𝑎, Poisson’s ratio ca, can be defined in card 4, col. 7, default = PRBA 𝜈𝑐𝑏, Poisson’s ratio cb, can be defined in card 4, col. 8, default = PRBA TAU1 *MAT_LAMINATED_COMPOSITE_FABRIC DESCRIPTION 𝜏1, stress limit of the first slightly nonlinear part of the shear stress versus shear strain curve. The values 𝜏1 and 𝛾1 are used to define a curve of shear stress versus shear strain. These values are input if FS, defined below, is set to a value of -1. GAMMA1 𝛾1, strain limit of the first slightly nonlinear part of the shear stress versus engineering shear strain curve. GAB GT.0.0: 𝐺𝑎𝑏, shear modulus ab direction LT.0.0: Load curve ID or Table ID = (-GAB) Load Curve. When (-GAB) is equal to a Load curve ID, it is taken as defining the elastic shear stress vs. shear strain behavior in ab direction. Tabular Data. When (-GAB) is equal to a a Table ID, it defines for each strain rate value a Load curve ID giv- ing the elastic shear stress vs. shear strain behavior in ab direction. Logarithmically Defined Tables. If the first elastic shear stress vs. shear strain curve in the table corre- sponds to a negative strain rate, LS-DYNA assumes that the natural logarithm of the strain rate value is used for all shear stress-shear strain curves. GBC GCA SLIMT1 SLIMC1 SLIMT2 SLIMC2 SLIMS 𝐺𝑏𝑐, shear modulus 𝑏𝑐 𝐺𝑐𝑎, shear modulus 𝑐𝑎 Factor to determine the minimum stress limit after stress maximum (fiber tension). Factor to determine the minimum stress limit after stress maximum (fiber compression). Factor to determine the minimum stress limit after stress maximum (matrix tension). Factor to determine the minimum stress limit after stress maximum (matrix compression). Factor to determine the minimum stress limit after stress maximum (shear). AOPT Material axes option (see MAT_OPTION TROPIC_ELASTIC for a VARIABLE DESCRIPTION more complete description): EQ.0.0: locally orthotropic with material axes determined by element nodes 1, 2, and 4, as with *DEFINE_COORDI- NATE_NODES, and then rotated about the shell ele- ment normal by an angle BETA. EQ.2.0: globally orthotropic with material axes determined by vectors defined below, as with *DEFINE_COORDI- NATE_VECTOR. EQ.3.0: locally orthotropic material axes determined by rotating the material axes about the element normal by an angle (BETA) from a line in the plane of the element defined by the cross product of the vector 𝐯 with the element normal. LT.0.0: the absolute value of AOPT is a coordinate system ID number (CID on *DEFINE_COORDINATE_NODES, *DEFINE_COORDINATE_SYSTEM or *DEFINE_CO- ORDINATE_VECTOR). TSIZE Time step for automatic element deletion. ERODS Maximum effective strain for element layer failure. A value of unity would equal 100% strain. GT.0.0: fails when effective strain calculated assuming material is volume preserving exceeds ERODS (old way). LT.0.0: fails when effective strain calculated from the full strain tensor exceeds |ERODS|. SOFT Softening reduction factor for strength in the crashfront. transverse shear stiffness GBC, GCA D = 0 D = TSMD EPSF EPSR transverse shear strain Figure M58-1. Linear Damage for transverse shear behavior VARIABLE DESCRIPTION FS Failure surface type: EQ.1.0: smooth failure surface with a quadratic criterion for both the fiber (a) and transverse (b) directions. This option can be used with complete laminates and fab- rics. EQ.0.0: smooth failure surface in the transverse (b) direction with a limiting value in the fiber (a) direction. This model is appropriate for unidirectional (UD) layered composites only. EQ.-1.: faceted failure surface. When the strength values are reached then damage evolves in tension and compres- sion for both the fiber and transverse direction. Shear behavior is also considered. This option can be used with complete laminates and fabrics. EPSF EPSR Damage initiation transverse shear strain. Final rupture transverse shear strain. TSMD Transverse shear maximum damage, default = 0.90. XP, YP, ZP Define coordinates of point 𝐩 for AOPT = 1. A1, A2, A3 Define components of vector 𝐚 for AOPT = 2. V1, V2 V3 Define components of vector 𝐯 for AOPT = 3. D1, D2, D3 Define components of vector 𝐝 for AOPT = 2. VARIABLE BETA E11C E11T E22C E22T GMS XC XT YC YT SC LCXC LCXT LCYC LCYT DESCRIPTION Material angle in degrees for AOPT = 0 and AOPT = 3. BETA may be overridden on the element card, see *ELEMENT_- SHELL_BETA. Strain at longitudinal compressive strength, 𝑎-axis (positive). Strain at longitudinal tensile strength, 𝑎-axis. Strain at transverse compressive strength, 𝑏-axis. Strain at transverse tensile strength, 𝑏-axis. Engineering shear strain at shear strength, 𝑎𝑏 plane. Longitudinal compressive strength (positive value). Longitudinal tensile strength, see below. Transverse compressive strength, 𝑏-axis (positive value), see below. Transverse tensile strength, 𝑏-axis, see below. Shear strength, 𝑎𝑏 plane, see below. Load curve ID defining longitudinal compressive strength XC vs. strain rate (XC is ignored with that option). If the first strain rate value in the curve is negative, it is assumed that all strain rate values are given as natural logarithm of the strain rate. Load curve ID defining longitudinal tensile strength XT vs. strain rate (XT is ignored with that option) If the first strain rate value in the curve is negative, it is assumed that all strain rate values are given as natural logarithm of the strain rate. Load curve ID defining transverse compressive strength YC vs. strain rate (YC is ignored with that option) If the first strain rate value in the curve is negative, it is assumed that all strain rate values are given as natural logarithm of the strain rate. Load curve ID defining transverse tensile strength YT vs. strain rate (YT is ignored with that option) If the first strain rate value in the curve is negative, it is assumed that all strain rate values are given as natural logarithm of the strain rate. LCSC LCTAU LCGAM *MAT_LAMINATED_COMPOSITE_FABRIC DESCRIPTION Load curve ID defining shear strength SC vs. strain rate (SC is ignored with that option) If the first strain rate value in the curve is negative, it is assumed that all strain rate values are given as natural logarithm of the strain rate. Load curve ID defining TAU1 vs. strain rate (TAU1 is ignored with that option). This value is only used for FS = -1. If the first strain rate value in the curve is negative, it is assumed that all strain rate values are given as natural logarithm of the strain rate. Load curve ID defining GAMMA1 vs. strain rate (GAMMA1 is ignored with that option). This value is only used for FS = -1. If the first strain rate value in the curve is negative, it is assumed that all strain rate values are given as natural logarithm of the strain rate. DT Strain rate averaging option. EQ.0.0: Strain rate is evaluated using a running average. LT.0.0: Strain rate is evaluated using average of last 11 time steps. GT.0.0: Strain rate is averaged over the last DT time units. Load curve ID defining E11C vs. strain rate (E11C is ignored with that option) If the first strain rate value in the curve is negative, it is assumed that all strain rate values are given as natural logarithm of the strain rate. Load curve ID defining E11T vs. strain rate (E11T is ignored with that option) If the first strain rate value in the curve is negative, it is assumed that all strain rate values are given as natural logarithm of the strain rate. Load curve ID defining E22C vs. strain rate (E22C is ignored with that option) If the first strain rate value in the curve is negative, it is assumed that all strain rate values are given as natural logarithm of the strain rate. Load curve ID defining E22T vs. strain rate (E22T is ignored with that option) If the first strain rate value in the curve is negative, it is assumed that all strain rate values are given as natural logarithm of the strain rate. LCE11C LCE11T LCE22C LCE22T DESCRIPTION Load curve ID defining GMS vs. strain rate (GMS is ignored with that option) If the first strain rate value in the curve is negative, it is assumed that all strain rate values are given as natural logarithm of the strain rate. Load curve ID defining ERODS vs. strain rate (ERODS is ignored with that option). The full strain tensor is used to compute the equivalent strain (new option). If the first strain rate value in the curve is negative, it is assumed that all strain rate values are given as natural logarithm of the strain rate. VARIABLE LCGMS LCEFS Remarks: Parameters to control failure of an element layer are: ERODS, the maximum effective strain, i.e., maximum 1 = 100% straining. The layer in the element is completely removed after the maximum effective strain (compression/tension including shear) is reached. The stress limits are factors used to limit the stress in the softening part to a given value, 𝜎min = SLIM𝑥𝑥 × strength, thus, the damage value is slightly modified such that elastoplastic like behavior is achieved with the threshold stress. The SLIMxx fields may range between 0.0 and 1.0. With a factor of 1.0, the stress remains at a maximum value identical to the strength, which is similar to ideal elastoplastic behavior. For tensile failure a small value for SLIMTx is often reasonable; however, for compression SLIMCx = 1.0 is preferred. This is also valid for the corresponding shear value. If SLIMxx is smaller than 1.0, then localization can be observed depending on the total behavior of the lay-up. If the user is intentionally using SLIMxx < 1.0, it is generally recommended to avoid a drop to zero and set the value to something in between 0.05 and 0.10. Then elastoplastic behavior is achieved in the limit which often leads to less numerical problems. Defaults for SLIM𝑥𝑥 = 10−8. The crashfront-algorithm is started if and only if a value for TSIZE is input. Note that time step size, with element elimination after the actual time step becomes smaller than TSIZE. The damage parameters can be written to the post processing database for each integration point as the first three additional element variables and can be visualized. τ TAU1 SC GAMMA1 GMS SLIMS = 1.0 SLIMS = 0.9 SLIMS = 0.6 γ Figure M58-2. Stress-strain diagram for shear Material models with FS = 1 or FS = -1 are favorable for complete laminates and fabrics, as all directions are treated in a similar fashion. For material model FS = 1 an interaction between normal stresses and the shear stresses is assumed for the evolution of damage in the a and b-directions. For the shear damage is always the maximum value of the damage from the criterion in a or b-direction is taken. For material model FS = -1 it is assumed that the damage evolution is independent of any of the other stresses. A coupling is only present via the elastic material parameters and the complete structure. In tensile and compression directions and in a as well as in b- direction different failure surfaces can be assumed. The damage values, however, increase only also when the loading direction changes. Special control of shear behavior of fabrics: For fabric materials a nonlinear stress strain curve for the shear part for failure surface FS = -1 can be assumed as given below. This is not possible for other values of FS. The curve, shown in Figure M58-2 is defined by three points: 1. 2. 3. the origin (0,0) is assumed, the limit of the first slightly nonlinear part (must be input), stress (TAU1) and strain (GAMMA1), see below. the shear strength at failure and shear strain at failure. In addition a stress limiter can be used to keep the stress constant via the SLIMS parameter. This value must be less or equal 1.0 but positive, and leads to an elastoplastic behavior for the shear part. The default is 10−8, assuming almost brittle failure once the strength limit SC is reached. *MAT_COMPOSITE_FAILURE_{OPTION}_MODEL This is Material Type 59. Available options include: SHELL SOLID SPH depending on the element type the material is to be used with, see *PART. Card 1 1 Variable MID Type A8 Card 2 1 2 RO F 2 3 EA F 3 Variable GAB GBC GCA Type F F F Card 3 Variable 1 XP Type F Card 4 Variable 1 V1 Type F 2 YP F 2 V2 F 3 ZP F 3 V3 F 4 EB F 4 KF F 4 A1 F 4 D1 F 5 EC F 5 6 7 8 PRBA PRCA PRCB F 6 F 7 F 8 AOPT MACF F I 5 A2 F 5 D2 F 6 A3 F 6 D3 F 7 8 7 8 BETA Card 5 for SHELL Keyword Option. Card 5 1 2 3 4 Variable TSIZE ALP SOFT FBRT Type F F F F Card 6 for SHELL Keyword Option. Card 6 Variable 1 XC Type F 2 XT F 3 YC F 4 YT F 5 SR F 5 SC F 7 8 6 SF F 6 7 8 Card 5 for SPH and SOLID Keyword Options. Card 5 1 2 3 4 5 6 7 8 Variable SBA SCA SCB XXC YYC ZZC Type F F F F F F Card 6 for SPH and SOLID Keyword Options. Card 6 1 2 3 4 5 6 7 8 Variable XXT YYT ZZT Type F F F VARIABLE DESCRIPTION MID RO EA Material identification. A unique number or label not exceeding 8 characters must be specified. Density 𝐸𝑎, Young’s modulus - longitudinal direction EB EC PRBA PRCA PRCB GAB GBC GCA KF AOPT *MAT_COMPOSITE_FAILURE_{OPTION}_MODEL DESCRIPTION 𝐸𝑏, Young’s modulus - transverse direction 𝐸𝑐, Young’s modulus - normal direction 𝜈𝑏𝑎, Poisson’s ratio ba 𝜈𝑐𝑎, Poisson’s ratio ca 𝜈𝑐𝑏, Poisson’s ratio cb 𝐺𝑎𝑏, Shear Modulus 𝐺𝑏𝑐, Shear Modulus 𝐺𝑐𝑎, Shear Modulus Bulk modulus of failed material Material axes option (SPH particles only support AOPT = 2.0): EQ.0.0: locally orthotropic with material axes determined by element nodes 1, 2, and 4, as with *DEFINE_COORDI- NATE_NODES, and then, for shells only, rotated about the shell element normal by an angle BETA. EQ.1.0: locally orthotropic with material axes determined by a point in space and the global location of the element center; this is the 𝑎-direction. This option is for solid elements only. EQ.2.0: globally orthotropic with material axes determined by vectors defined below, as with *DEFINE_COORDI- NATE_VECTOR. EQ.3.0: locally orthotropic material axes determined by rotating the material axes about the element normal by an angle, BETA, from a line in the plane of the element defined by the cross product of the vector 𝐯 with the element normal. EQ.4.0: locally orthotropic in cylindrical coordinate system with the material axes determined by a vector 𝐯, and an originating point, 𝐩, which define the centerline ax- is. This option is for solid elements only. LT.0.0: the absolute value of AOPT is a coordinate system ID VARIABLE DESCRIPTION number (CID on *DEFINE_COORDINATE_NODES, *DEFINE_COORDINATE_SYSTEM or *DEFINE_CO- ORDINATE_VECTOR). Available in R3 version of 971 and later. MACF Material axes change flag for brick elements. EQ.1: No change, default, EQ.2: switch material axes 𝑎 and 𝑏, EQ.3: switch material axes 𝑎 and 𝑐, EQ.4: switch material axes 𝑏 and 𝑐. XP YP ZP Define coordinates of point 𝐩 for AOPT = 1 and 4. A1 A2 A3 Define components of vector 𝐚 for AOPT = 2. V1 V2 V3 Define components of vector 𝐯 for AOPT = 3 and 4. D1 D2 D3 Define components of vector 𝐝 for AOPT = 2: BETA Material angle in degrees for AOPT = 0 (shells only) and AOPT = 3, may be overridden on the element card, see *ELE- MENT_SHELL_BETA or *ELEMENT_SOLID_ORTHO. TSIZE Time step for automatic element deletion ALP SOFT FBRT SR SF XC XT YC YT Nonlinear shear stress parameter Softening reduction factor for strength in crush Softening of fiber tensile strength 𝑠𝑟, reduction factor (default = 0.447) 𝑠𝑓 , softening factor (default = 0.0) Longitudinal compressive strength, 𝑎-axis (positive value). Longitudinal tensile strength, 𝑎-axis Transverse compressive strength, 𝑏-axis (positive value). Transverse tensile strength, 𝑏-axis *MAT_COMPOSITE_FAILURE_{OPTION}_MODEL DESCRIPTION SC Shear strength, 𝑎𝑏 plane: GT.0.0: faceted failure surface theory, LT.0.0: ellipsoidal failure surface theory. SBA SCA SCB XXC YYC ZZC XXT YYT ZZT In plane shear strength. Transverse shear strength. Transverse shear strength. Longitudinal compressive strength 𝑎-axis (positive value). Transverse compressive strength 𝑏-axis (positive value). Normal compressive strength 𝑐-axis (positive value). Longitudinal tensile strength 𝑎-axis. Transverse tensile strength 𝑏-axis. Normal tensile strength 𝑐-axis. *MAT_ELASTIC_WITH_VISCOSITY This is Material Type 60 which was developed to simulate forming of glass products (e.g., car windshields) at high temperatures. Deformation is by viscous flow but elastic deformations can also be large. The material model, in which the viscosity may vary with temperature, is suitable for treating a wide range of viscous flow problems and is implemented for brick and shell elements. Card 1 1 Variable MID Type A8 Card 2 1 2 RO F 2 3 V0 F 3 4 A F 4 5 B F 5 6 C F 6 7 8 LCID F 7 8 Variable PR1 PR2 PR3 PR4 PR5 PR6 PR7 PR8 Type F F F F F F F F Card 3 Variable 1 T1 Type F Card 4 Variable 1 V1 Type F 2 T2 F 2 V2 F 3 T3 F 3 V3 F 4 T4 F 4 V4 F 5 T5 F 5 V5 F 6 T6 F 6 V6 F 7 T7 F 7 V7 F 8 T8 F 8 V8 Variable 1 E1 Type F Card 6 1 *MAT_ELASTIC_WITH_VISCOSITY 2 E2 F 2 3 E3 F 3 4 E4 F 4 5 E5 F 5 6 E6 F 6 7 E7 F 7 8 E8 F 8 Variable ALPHA1 ALPHA2 ALPHA3 ALPHA4 ALPHA5 ALPHA6 ALPHA7 ALPHA8 Type F F F F F F F F VARIABLE DESCRIPTION MID RO V0 A B C LCID T1, T2, …, TN PR1, PR2, …, PRN V1, V2, …, VN 2-346 (EOS) Material identification. A unique number or label not exceeding 8 characters must be specified. Mass density Temperature independent dynamic viscosity coefficient, V0. If defined, the temperature dependent viscosity defined below is skipped, see type (i) and (ii) definitions for viscosity below. Dynamic viscosity coefficient, see type (i) and (ii) definitions below. Dynamic viscosity coefficient, see type (i) and (ii) definitions below. Dynamic viscosity coefficient, see type (i) and (ii) definitions below. Load curve defining viscosity versus temperature, see type (iii). (Optional) Temperatures, define up to 8 values Poisson’s ratios for the temperatures Ti Corresponding dynamic viscosity coefficients (define only one if VARIABLE DESCRIPTION E1, E2, …, EN Corresponding Young’s moduli coefficients (define only one if not varying with temperature) Corresponding thermal expansion coefficients ALPHA1, …, ALPHAN. Remarks: Volumetric behavior is treated as linear elastic. The deviatoric strain rate is considered to be the sum of elastic and viscous strain rates: ′ = 𝛆̇elastic 𝛆̇total ′ ′ + 𝛆̇viscous = 𝛔̇′ 2𝐺 + 𝛔′ 2𝜈 where G is the elastic shear modulus, v is the viscosity coefficient, and bold indicates a tensor. The stress increment over one timestep dt is 𝑑𝜎 ′ = 2𝐺𝜺̇total𝑑𝑡 − 𝑑𝑡 σ′ The stress before the update is used for σ′. For shell elements the through-thickness strain rate is calculated as follows. 𝑑𝜎33 = 0 = 𝐾(𝜀̇11 + 𝜀̇22 + 𝜀̇33)𝑑𝑡 + 2𝐺𝜀′̇ 33𝑑𝑡 − 𝑑𝑡𝜎′33 where the subscript ij = 33 denotes the through-thickness direction and K is the elastic bulk modulus. This leads to: 𝐺) 𝑎 = 𝜀̇33 = −𝑎(𝜀̇11 + 𝜀̇22) + 𝑏𝑝 (𝐾 − 2 (𝐾 + 4 𝐺𝑑𝑡 𝜐(𝐾 + 4 𝑏 = 𝐺) 𝐺) in which p is the pressure defined as the negative of the hydrostatic stress. The variation of viscosity with temperature can be defined in any one of the 3 ways. (i) Constant, V = V0 Do not define constants, A, B, and C or the piecewise curve.(leave card 4 blank) (ii) V = V0 × 10 (A/(T-B) + C) (iii) Piecewise curve: define the variation of viscosity with temperature. NOTE: Viscosity is inactive during dynamic re- laxation. *MAT_ELASTIC_WITH_VISCOSITY_CURVE This is Material Type 60 which was developed to simulate forming of glass products (e.g., car windshields) at high temperatures. Deformation is by viscous flow but elastic deformations can also be large. The material model, in which the viscosity may vary with temperature, is suitable for treating a wide range of viscous flow problems and is implemented for brick and shell elements. Load curves are used to represent the temperature dependence of Poisson’s ratio, Young’s modulus, the coefficient of expansion, and the viscosity. Card 1 1 Variable MID Type A8 Card 2 1 2 RO F 2 3 V0 F 3 4 A F 4 5 B F 5 6 C F 6 7 8 LCID F 7 8 Variable PR_LC YM_LC A_LC V_LC V_LOG Type F F F F F VARIABLE DESCRIPTION MID RO V0 A B C Material identification. A unique number or label not exceeding 8 characters must be specified. Mass density Temperature independent dynamic viscosity coefficient, V0. If defined, the temperature dependent viscosity defined below is skipped, see type (i) and (ii) definitions for viscosity below. Dynamic viscosity coefficient, see type (i) and (ii) definitions below. Dynamic viscosity coefficient, see type (i) and (ii) definitions below. Dynamic viscosity coefficient, see type (i) and (ii) definitions below. VARIABLE DESCRIPTION Load curve defining factor on dynamic viscosity versus temperature, see type (iii). (Optional). Load curve defining Poisson’s ratio as a function of temperature. Load curve defining Young’s modulus as a function of temperature. Load curve defining the coefficient of thermal expansion as a function of temperature. Load curve defining the dynamic viscosity as a function of temperature. Flag for the form of V_LC. If V_LOG = 1.0, the value specified in V_LC is the natural logarithm of the viscosity, ln(V). The value interpolated from the curve is then exponentiated to obtain the viscosity. If V_LOG = 0.0, the value is the viscosity. The logarithmic form is useful if the value of the viscosity changes by orders of magnitude over the temperature range of the data. LCID PR_LC YM_LC A_LC V_LC V_LOG Remarks: Volumetric behavior is treated as linear elastic. The deviatoric strain rate is considered to be the sum of elastic and viscous strain rates: ′ = ε̇elastic ε̇total ′ ′ + ε̇viscous = 𝝈̇ ′ 2𝐺 + σ′ 2𝜈 where G is the elastic shear modulus, v is the viscosity coefficient, and bold~ indicates a tensor. The stress increment over one timestep dt is 𝑑𝝈′ = 2𝐺ε̇total ′ 𝑑𝑡 − 𝑑𝑡 𝝈′ The stress before the update is used for σ′. For shell elements the through-thickness strain rate is calculated as follows. 𝑑𝜎33 = 0 = 𝐾(𝜀̇11 + 𝜀̇22 + 𝜀̇33)𝑑𝑡 + 2𝐺𝜀′̇ 33𝑑𝑡 − 𝑑𝑡𝜎′33 where the subscript ij = 33 denotes the through-thickness direction and K is the elastic bulk modulus. This leads to: 𝜀̇33 = −𝑎(𝜀̇11 + 𝜀̇22) + 𝑏𝑝 𝑎 = 𝑏 = 𝐺) 𝐺) (𝐾 − 2 (𝐾 + 4 𝐺𝑑𝑡 𝜐(𝐾 + 4 𝐺) in which p is the pressure defined as the negative of the hydrostatic stress. The variation of viscosity with temperature can be defined in any one of the 3 ways. (i) (ii) (iii) Constant, V = V0 Do not define constants, A, B, and C or the piecewise curve.(leave card 4 blank) V = V0 × 10(A/(T-B) + C) Piecewise curve: define the variation of viscosity with temperature. Note: Viscosity is inactive during dynamic relaxation. *MAT_KELVIN-MAXWELL_VISCOELASTIC This is Material Type 61. This material is a classical Kelvin-Maxwell model for modeling viscoelastic bodies, e.g., foams. This model is valid for solid elements only. See also notes below. Card 1 1 Variable MID 2 RO 3 BULK Type A8 F F 4 G0 F 5 GI F 6 DC F 7 FO F 8 SO F Default none none none none none 0.0 0.0 0.0 VARIABLE MID DESCRIPTION Material identification. A unique number or label not exceeding 8 characters must be specified. RO Mass density BULK Bulk modulus (elastic) G0 GI DC FO Short-time shear modulus, G0 Long-time (infinite) shear modulus, G∞ Maxwell decay constant, β[FO = 0.0] or Kelvin relaxation constant, τ [FO = 1.0] Formulation option: EQ.0.0: Maxwell, EQ.1.0: Kelvin. VARIABLE SO DESCRIPTION Strain (logarithmic) output option to control what is written as component 7 to the d3plot database. (LS-PrePost always blindly labels this component as effective plastic strain.) The maximum values are updated for each element each time step: EQ.0.0: maximum principal strain that occurs during the calculation, EQ.1.0: maximum magnitude of the principal strain values that occurs during the calculation, EQ.2.0: maximum effective strain that occurs during the calculation. Remarks: The shear relaxation behavior is described for the Maxwell model by: A Jaumann rate formulation is used 𝐺(𝑡) = 𝐺 + (𝐺0 − 𝐺∞)𝑒−𝛽𝑡 ∇ ′ = 2 ∫ 𝐺(𝑡 − 𝜏) 𝐷′𝑖𝑗(𝜏)𝑑𝑡 ij 𝑡 0 ∇ 𝑖𝑗, and the strain rate Dij . where the prime denotes the deviatoric part of the stress rate, 𝜎 For the Kelvin model the stress evolution equation is defined as: 𝑠 ̇𝑖𝑗 + 𝑠𝑖𝑗 = (1 + 𝛿𝑖𝑗)𝐺0𝑒 ̇𝑖𝑗 + (1 + 𝛿𝑖𝑗) 𝐺∞ 𝑒 ̇𝑖𝑗 The strain data as written to the LS-DYNA database may be used to predict damage, see [Bandak 1991]. *MAT_VISCOUS_FOAM This is Material Type 62. It was written to represent the Confor Foam on the ribs of EuroSID side impact dummy. It is only valid for solid elements, mainly under compressive loading. Card 1 1 Variable MID 2 RO Type A8 F 3 E1 F 4 N1 F 5 V2 F 6 E2 F 7 N2 F 8 PR F VARIABLE MID DESCRIPTION Material identification. A unique number or label not exceeding 8 characters must be specified. Mass density Initial Young’s modulus (E1) Exponent in power law for Young’s modulus (n1) Viscous coefficient (V2) Elastic modulus for viscosity (E2), see notes below. Exponent in power law for viscosity (n2) Poisson’s ratio, ν RO E1 N1 V2 E2 N2 PR Remarks: The model consists of a nonlinear elastic stiffness in parallel with a viscous damper. The elastic stiffness is intended to limit total crush while the viscosity absorbs energy. The stiffness E2 exists to prevent timestep problems. It is used for time step calculations 𝑡 is smaller than E2. It has to be carefully chosen to take into account the a long as 𝐸1 stiffening effects of the viscosity. Both E1 and V2 are nonlinear with crush as follows: 𝑡 = 𝐸1(𝑉−𝑛1) 𝐸1 𝑡 = 𝑉2|1 − 𝑉|𝑛2 𝑉2 where viscosity generates a shear stress given by 𝛾̇ is the engineering shear strain rate, and V is the relative volume defined by the ratio of the current to initial volume. 𝜏 = 𝑉2𝛾̇ Table showing typical values (units of N, mm, s): Card 1 1 Variable MID 2 RO 3 E1 4 N1 5 V2 6 E2 7 N2 8 PR Value 0.0036 4.0 0.0015 100.0 0.2 0.05 *MAT_CRUSHABLE_FOAM This is Material Type 63 which is dedicated to modeling crushable foam with optional damping and tension cutoff. Unloading is fully elastic. Tension is treated as elastic- perfectly-plastic at the tension cut-off value. A modified version of this model, *MAT_- MODIFIED_CRUSHABLE_FOAM includes strain rate effects. Card 1 1 Variable MID 2 RO Type A8 F 3 E F 4 PR F 5 6 7 8 LCID TSC DAMP F F F Default none none none none none 0.0 0.10 VARIABLE DESCRIPTION MID RO E PR LCID TSC Material identification. A unique number or label not exceeding 8 characters must be specified. Mass density Young’s modulus Poisson’s ratio Load curve ID defining yield stress versus volumetric strain, 𝛾, see Figure M63-1. Tensile stress cutoff. A nonzero, positive value is strongly recommended for realistic behavior. DAMP Rate sensitivity via damping coefficient (.05 < recommended value < .50). Stress increases at higher strain rates Volumetric Strain Figure M63-1. Behavior of strain rate sensitive crushable foam. Unloading is elastic to the tension cutoff. Subsequent reloading follows the unloading curve Remarks: The volumetric strain is defined in terms of the relative volume, V, as: 𝛾 = 1 − 𝑉 The relative volume is defined as the ratio of the current to the initial volume. In place of the effective plastic strain in the d3plot database, the integrated volumetric strain (natural logarithm of the relative volume) is output. *MAT_RATE_SENSITIVE_POWERLAW_PLASTICITY This is Material Type 64 which will model strain rate sensitive elasto-plastic material with a power law hardening. Optionally, the coefficients can be defined as functions of the effective plastic strain. Card 1 1 Variable MID 2 RO Type A8 F 3 E F 4 PR F 5 K F 6 M F 7 N F 8 E0 F Default none none none none none 0.0001 none 0.0002 Card 2 Variable 1 VP 2 3 4 5 6 7 8 EPS0 Type F F Default 0.0 1.0 VARIABLE MID DESCRIPTION Material identification. A unique number or label not exceeding 8 characters must be specified. RO E PR K M Mass density Young’s modulus of elasticity Poisson’s ratio Material constant, k. If k < 0 the absolute value of k is taken as the load curve number that defines k as a function of effective plastic strain. Strain hardening coefficient, m. If m < 0 the absolute value of m is taken as the load curve number that defines m as a function of effective plastic strain. VARIABLE DESCRIPTION N E0 VP Strain rate sensitivity coefficient, n. If n < 0 the absolute value of n is taken as the load curve number that defines n as a function of effective plastic strain. Initial strain rate (default = 0.0002) Formulation for rate effects: EQ.0.0: Scale yield stress (default) EQ.1.0: Viscoplastic formulation EPS0 Quasi-static threshold strain rate. See description under *MAT_- 015. Remarks: This material model follows a constitutive relationship of the form: 𝜎 = 𝑘𝜀𝑚𝜀̇𝑛 where 𝜎 is the yield stress, 𝜀 is the effective plastic strain, 𝜀̇ is the effective total strain rate (VP = 0), respectively the effective plastic strain rate (VP = 1), and the constants k, m, and n can be expressed as functions of effective plastic strain or can be constant with respect to the plastic strain. The case of no strain hardening can be obtained by setting the exponent of the plastic strain equal to a very small positive value, i.e. 0.0001. This model can be combined with the superplastic forming input to control the magnitude of the pressure in the pressure boundary conditions in order to limit the effective plastic strain rate so that it does not exceed a maximum value at any integration point within the model. A fully viscoplastic formulation is optional. An additional cost is incurred but the improvement is results can be dramatic. *MAT_MODIFIED_ZERILLI_ARMSTRONG This is Material Type 65 which is a rate and temperature sensitive plasticity model which is sometimes preferred in ordnance design calculations. Card 1 1 Variable MID 2 RO Type A8 F Card 2 Variable 1 C1 Type F Card 3 Variable 1 B1 Type F 2 C2 F 2 B2 F 3 G F 3 C3 F 3 B3 F 4 E0 F 4 C4 F 4 G1 F 5 N F 5 C5 F 5 G2 F 6 7 8 TROOM PC SPALL F 6 C6 F 6 G3 F F 8 VP F 8 BULK F 7 EFAIL F 7 G4 F VARIABLE DESCRIPTION MID RO G E0 N Material identification. A unique number or label not exceeding 8 characters must be specified. Mass density Shear modulus 𝜀̇0, factor to normalize strain rate n, exponent for bcc metal TROOM Tr, room temperature PC pc, Pressure cutoff VARIABLE DESCRIPTION SPALL Spall Type: EQ.1.0: minimum pressure limit, EQ.2.0: maximum principal stress, EQ.3.0: minimum pressure cutoff. C1, coefficients for flow stress, see notes below. C2, coefficients for flow stress, see notes below. C3, coefficients for flow stress, see notes below. C4, coefficients for flow stress, see notes below. C5, coefficients for flow stress, see notes below. C6, coefficients for flow stress, see notes below. C1 C2 C3 C4 C5 C6 EFAIL Failure strain for erosion VP Formulation for rate effects: EQ.0.0: Scale yield stress (default) EQ.1.0: Viscoplastic formulation B1 B2 B3 G1 G2 G3 G4 B1, coefficients dependency of flow stress yield. for polynomial to represent temperature B2 B3 G1, coefficients for defining heat capacity and temperature dependency of heat capacity. G2 G3 G4 BULK Bulk modulus defined for shell elements only. Do not input for solid elements. *MAT_MODIFIED_ZERILLI_ARMSTRONG The Armstrong-Zerilli Material Model expresses the flow stress as follows. For fcc metals (n = 0), 𝜎 = 𝐶1 + {𝐶2(𝜀𝑝) 2⁄ [𝑒[−𝐶3+𝐶4ln(𝜀̇∗)]𝑇] + 𝐶5} [ 𝜇(𝑇) 𝜇(293) ] where, 𝜀𝑝 = effective plastic strain 𝜀̇∗ = effective plastic strain rate = 𝜀̇ 𝜀̇0 and 𝜀̇0 = 1, 1e-3, 1e-6 for time units of seconds, milliseconds, and microseconds, respectively. For bcc metals (n > 0), 𝜎 = 𝐶1 + 𝐶2𝑒[−𝐶3+𝐶4ln(𝜀̇∗)]𝑇 + [𝐶5(𝜀𝑝)𝑛 + 𝐶6] [ 𝜇(𝑇) 𝜇(293) ] where 𝜇(𝑇) 𝜇(293) = 𝐵1 + 𝐵2𝑇 + 𝐵3𝑇2. The relationship between heat capacity (specific heat) and temperature may be characterized by a cubic polynomial equation as follows: 𝐶𝑝 = 𝐺1 + 𝐺2𝑇 + 𝐺3𝑇2 + 𝐺4𝑇3 A fully viscoplastic formulation is optional. An additional cost is incurred but the improvement is results can be dramatic. *MAT_LINEAR_ELASTIC_DISCRETE_BEAM This is Material Type 66. This material model is defined for simulating the effects of a linear elastic beam by using six springs each acting about one of the six local degrees-of- freedom. The two nodes defining a beam may be coincident to give a zero length beam, or offset to give a finite length beam. For finite length discrete beams the absolute value of the variable SCOOR in the SECTION_BEAM input should be set to a value of 2.0, which causes the local r-axis to be aligned along the two nodes of the beam to give physically correct behavior. The distance between the nodes of a beam should not affect the behavior of this model. A triad is used to orient the beam for the directional springs. Translational/rotational stiffness and viscous damping effects are considered for a local cartesian system, see notes below. Applications for this element include the modeling of joint stiffnesses. Card 1 1 Variable MID Type A8 Card 2 1 2 RO F 2 3 4 5 6 7 8 TKR TKS TKT RKR RKS RKT F 3 F 4 F 5 F 6 F 7 F 8 Variable TDR TDS TDT RDR RDS RDT Type F Card 3 1 F 2 F 3 F 4 F 5 F 6 7 8 Variable FOR FOS FOT MOR MOS MOT Type F F F F F F VARIABLE DESCRIPTION MID RO Material identification. A unique number or label not exceeding 8 characters must be specified. Mass density, see also “volume” in the *SECTION_BEAM definition. *MAT_LINEAR_ELASTIC_DISCRETE_BEAM DESCRIPTION TKR TKS TKT RKR RKS RKT TDR TDS TDT RDR RDS RDT FOR FOS FOT MOR MOS MOT Translational stiffness along local r-axis, see notes below. Translational stiffness along local s-axis. Translational stiffness along local t-axis. Rotational stiffness about the local r-axis. Rotational stiffness about the local s-axis. Rotational stiffness about the local t-axis. Translational viscous damper along local r-axis. (Optional) Translational viscous damper along local s-axis. (Optional) Translational viscous damper along local t-axis. (Optional) Rotational viscous damper about the local r-axis. (Optional) Rotational viscous damper about the local s-axis. (Optional) Rotational viscous damper about the local t-axis. (Optional) Preload force in r-direction. (Optional) Preload force in s-direction. (Optional) Preload force in t-direction. (Optional) Preload moment about r-axis. (Optional) Preload moment about s-axis. (Optional) Preload moment about t-axis. (Optional) Remarks: The formulation of the discrete beam (type 6) assumes that the beam is of zero length and requires no orientation node. A small distance between the nodes joined by the beam is permitted. The local coordinate system which determines (r,s,t) is given by the coordinate ID, see *DEFINE_COORDINATE_OPTION, in the cross sectional input, see *SECTION_BEAM, where the global system is the default. The local coordinate system axes can rotate with either node of the beam or an average rotation of both nodes . For null stiffness coefficients, no forces corresponding to these null values will develop. The viscous damping coefficients are optional. *MAT_NONLINEAR_ELASTIC_DISCRETE_BEAM This is Material Type 67. This material model is defined for simulating the effects of nonlinear elastic and nonlinear viscous beams by using six springs each acting about one of the six local degrees-of-freedom. The two nodes defining a beam may be coincident to give a zero length beam, or offset to give a finite length beam. For finite length discrete beams the absolute value of the variable SCOOR in the SECTION_- BEAM input should be set to a value of 2.0, which causes the local r-axis to be aligned along the two nodes of the beam to give physically correct behavior. The distance between the nodes of a beam should not affect the behavior of this material model. A triad is used to orient the beam for the directional springs. Arbitrary curves to model transitional/ rotational stiffness and damping effects are allowed. See notes below. Card 1 1 2 3 4 5 6 7 8 Variable MID RO LCIDTR LCIDTS LCIDTT LCIDRR LCIDRS LCIDRT Type A8 Card 2 1 F 2 F 3 F 4 F 5 F 6 F 7 F 8 Variable LCIDTDR LCIDTDS LCIDTDT LCIDRDR LCIDRDS LCIDRDT Type F Card 3 1 F 2 F 3 F 4 F 5 F 6 7 8 Variable FOR FOS FOT MOR MOS MOT Type F F F F F Optional Failure Cards. Cards 4 and 5 must be defined to consider failure; otherwise, they are optional. Card 4 1 2 3 4 5 6 7 8 Variable FFAILR FFAILS FFAILT MFAILR MFAILS MFAILT Type F F F F F F Default 0.0 0.0 0.0 0.0 0.0 0.0 Card 5 1 2 3 4 5 6 7 8 Variable UFAILR UFAILS UFAILT TFAILR TFAILS TFAILT Type F F F F F F Default 0.0 0.0 0.0 0.0 0.0 0.0 VARIABLE MID DESCRIPTION Material identification. A unique number or label not exceeding 8 characters must be specified. RO Mass density, see also volume in *SECTION_BEAM definition. LCIDTR LCIDTS LCIDTT LCIDRR LCIDRS Load curve ID defining translational force resultant along local r- axis versus relative translational displacement, see Remarks and Figure M67-1. Load curve ID defining translational force resultant along local s- axis versus relative translational displacement. Load curve ID defining translational force resultant along local t- axis versus relative translational displacement. Load curve ID defining rotational moment resultant about local r- axis versus relative rotational displacement. Load curve ID defining rotational moment resultant about local s- axis versus relative rotational displacement. LCIDRT LCIDTDR LCIDTDS LCIDTDT LCIDRDR LCIDRDS LCIDRDT FOR FOS FOT MOR MOS MOT FFAILR FFAILS FFAILT MFAILR *MAT_NONLINEAR_ELASTIC_DISCRETE_BEAM DESCRIPTION Load curve ID defining rotational moment resultant about local t- axis versus relative rotational displacement. Load curve ID defining translational damping force resultant along local r-axis versus relative translational velocity. Load curve ID defining translational damping force resultant along local s-axis versus relative translational velocity. Load curve ID defining translational damping force resultant along local t-axis versus relative translational velocity. Load curve ID defining rotational damping moment resultant about local r-axis versus relative rotational velocity. Load curve ID defining rotational damping moment resultant about local s-axis versus relative rotational velocity. Load curve ID defining rotational damping moment resultant about local t-axis versus relative rotational velocity. Preload force in r-direction. (Optional) Preload force in s-direction. (Optional) Preload force in t-direction. (Optional) Preload moment about r-axis. (Optional) Preload moment about s-axis. (Optional) Preload moment about t-axis. (Optional) Optional failure parameter. If zero, the corresponding force, Fr, is not considered in the failure calculation. Optional failure parameter. If zero, the corresponding force, Fs, is not considered in the failure calculation. Optional failure parameter. If zero, the corresponding force, Ft, is not considered in the failure calculation. Optional failure parameter. If zero, the corresponding moment, Mr, is not considered in the failure calculation. DESCRIPTION Optional failure parameter. If zero, the corresponding moment, Ms, is not considered in the failure calculation. Optional failure parameter. If zero, the corresponding moment, Mt, is not considered in the failure calculation. Optional displacement, ur, is not considered in the failure calculation. failure parameter. If zero, the corresponding Optional displacement, us, is not considered in the failure calculation. failure parameter. If zero, the corresponding Optional displacement, ut, is not considered in the failure calculation. failure parameter. If zero, the corresponding Optional failure parameter. If zero, the corresponding rotation, θr, is not considered in the failure calculation. Optional failure parameter. If zero, the corresponding rotation, θs, is not considered in the failure calculation. Optional failure parameter. If zero, the corresponding rotation, θt, is not considered in the failure calculation. VARIABLE MFAILS MFAILT UFAILR UFAILS UFAILT TFAILR TFAILS TFAILT Remarks: For null load curve ID’s, no forces are computed. The formulation of the discrete beam (type 6) assumes that the beam is of zero length and requires no orientation node. A small distance between the nodes joined by the beam is permitted. The local coordinate system which determines (r,s,t) is given by the coordinate ID, see *DEFINE_COORDINATE_OPTION, in the cross sectional input, see *SECTION_BEAM, where the global system is the default. The local coordinate system axes can rotate with either node of the beam or an average rotation of both nodes . If different behavior in tension and compression is desired in the calculation of the force resultants, the load curve(s) must be defined in the negative quadrant starting with the most negative displacement then increasing monotonically to the most positive. If the load curve behaves similarly in tension and compression, define only the positive quadrant. Whenever displacement values fall outside of the defined range, the resultant forces will be extrapolated. Figure M67-1 depicts a typical load curve for a force resultant. Load curves used for determining the damping forces and moment resultants always act identically in tension and compression, since only the positive quadrant values are considered, i.e., start the load curve at the origin [0,0]. (a.) DISPLACEMENT (b.) Figure M67-1. The resultant forces and moments are determined by a table lookup. If the origin of the load curve is at [0,0] as in (b.) and tension and compression responses are symmetric. | DISPLACEMENT | Catastrophic failure based on force resultants occurs if the following inequality is satisfied. ( 𝐹𝑟 fail 𝐹𝑟 ) + ( 𝐹𝑠 fail 𝐹𝑠 ) + ( 𝐹𝑡 fail 𝐹𝑡 ) + ( 𝑀𝑟 fail 𝑀𝑟 ) + ( 𝑀𝑠 fail 𝑀𝑠 ) + ( 𝑀𝑡 fail 𝑀𝑡 ) − 1. ≥ 0. After failure the discrete element is deleted. Likewise, catastrophic failure based on displacement resultants occurs if the following inequality is satisfied: ( 𝑢𝑟 fail 𝑢𝑟 ) + ( 𝑢𝑠 fail 𝑢𝑠 ) + ( 𝑢𝑡 fail 𝑢𝑡 ) + ( ) 𝜃𝑟 fail 𝜃𝑟 + ( 𝜃𝑠 fail 𝜃𝑠 ) + ( 𝜃𝑡 fail 𝜃𝑡 ) − 1. ≥ 0. After failure the discrete element is deleted. If failure is included either one or both of the criteria may be used. *MAT_NONLINEAR_PLASTIC_DISCRETE_BEAM This is Material Type 68. This material model is defined for simulating the effects of nonlinear elastoplastic, linear viscous behavior of beams by using six springs each acting about one of the six local degrees-of-freedom. The two nodes defining a beam may be coincident to give a zero length beam, or offset to give a finite length beam. For finite length discrete beams the absolute value of the variable SCOOR in the SEC- TION_BEAM input should be set to a value of 2.0, which causes the local r-axis to be aligned along the two nodes of the beam to give physically correct behavior. The distance between the nodes of a beam should not affect the behavior of this material model. A triad is used to orient the beam for the directional springs. Translation- al/rotational stiffness and damping effects can be considered. The plastic behavior is modeled using force/moment curves versus displacements/rotation. Optionally, failure can be specified based on a force/moment criterion and a displacement rotation criterion. See also notes below. Card 1 1 Variable MID 2 RO 3 4 5 6 7 8 TKR TKS TKT RKR RKS RKT Type A8 F F F F F F F Default none none none none none none none none Card 2 1 2 3 4 5 6 7 8 Variable TDR TDS TDT RDR RDS RDT Type F F F F F F Default none none none none none none Card 3 1 2 3 4 5 6 7 8 Variable LCPDR LCPDS LCPDT LCPMR LCPMS LCPMT Type F F F F F F Default 0.0 0.0 0.0 0.0 0.0 0.0 Card 4 1 2 3 4 5 6 7 8 Variable FFAILR FFAILS FFAILT MFAILR MFAILS MFAILT Type F F F F F F Default 0.0 0.0 0.0 0.0 0.0 0.0 Card 5 1 2 3 4 5 6 7 8 Variable UFAILR UFAILS UFAILT TFAILR TFAILS TFAILT Type F F F F F F Default 0.0 0.0 0.0 0.0 0.0 0.0 Card 6 1 2 3 4 5 6 7 8 Variable FOR FOS FOT MOR MOS MOT Type F F F F F F VARIABLE MID DESCRIPTION Material identification. A unique number or label not exceeding 8 characters must be specified. RO Mass density, see also volume on *SECTION_BEAM definition. VARIABLE DESCRIPTION TKR TKS TKT RKR RKS RKT TDR TDS TDT RDR RDS RDT LCPDR LCPDS LCPDT LCPMR LCPMS Translational stiffness along local r-axis Translational stiffness along local s-axis Translational stiffness along local t-axis Rotational stiffness about the local r-axis Rotational stiffness about the local s-axis Rotational stiffness about the local t-axis Translational viscous damper along local r-axis Translational viscous damper along local s-axis Translational viscous damper along local t-axis Rotational viscous damper about the local r-axis Rotational viscous damper about the local s-axis Rotational viscous damper about the local t-axis Load curve ID-yield force versus plastic displacement r-axis. If the curve ID is zero, and if TKR is nonzero, then elastic behavior is obtained for this component. Load curve ID-yield force versus plastic displacement s-axis. If the curve ID is zero, and if TKS is nonzero, then elastic behavior is obtained for this component. Load curve ID-yield force versus plastic displacement t-axis. If the curve ID is zero, and if TKT is nonzero, then elastic behavior is obtained for this component. Load curve ID-yield moment versus plastic rotation r-axis. If the curve ID is zero, and if RKR is nonzero, then elastic behavior is obtained for this component. Load curve ID-yield moment versus plastic rotation s-axis. If the curve ID is zero, and if RKS is nonzero, then elastic behavior is obtained for this component. LCPMT FFAILR FFAILS FFAILT MFAILR MFAILS MFAILT UFAILR UFAILS UFAILT TFAILR TFAILS TFAILT FOR FOS *MAT_NONLINEAR_PLASTIC_DISCRETE_BEAM DESCRIPTION Load curve ID-yield moment versus plastic rotation t-axis. If the curve ID is zero, and if RKT is nonzero, then elastic behavior is obtained for this component. Optional failure parameter. If zero, the corresponding force, Fr, is not considered in the failure calculation. Optional failure parameter. If zero, the corresponding force, Fs, is not considered in the failure calculation. Optional failure parameter. If zero, the corresponding force, Ft, is not considered in the failure calculation. Optional failure parameter. If zero, the corresponding moment, Mr, is not considered in the failure calculation. Optional failure parameter. If zero, the corresponding moment, Ms, is not considered in the failure calculation. Optional failure parameter. If zero, the corresponding moment, Mt, is not considered in the failure calculation. Optional displacement, ur, is not considered in the failure calculation. failure parameter. If zero, the corresponding Optional displacement, us, is not considered in the failure calculation. failure parameter. If zero, the corresponding Optional displacement, ut, is not considered in the failure calculation. failure parameter. If zero, the corresponding Optional failure parameter. If zero, the corresponding rotation, θr, is not considered in the failure calculation. Optional failure parameter. If zero, the corresponding rotation, θs, is not considered in the failure calculation. Optional failure parameter. If zero, the corresponding rotation, θt, is not considered in the failure calculation. Preload force in r-direction. (Optional) Preload force in s-direction. (Optional) VARIABLE DESCRIPTION Preload force in t-direction. (Optional) Preload moment about r-axis. (Optional) Preload moment about s-axis. (Optional) Preload moment about t-axis. (Optional) FOT MOR MOS MOT Remarks: For the translational and rotational degrees of freedom where elastic behavior is desired, set the load curve ID to zero. The plastic displacement for the load curves is defined as: plastic displacement = total displacement − yield force/elastic stiffness The formulation of the discrete beam (type 6) assumes that the beam is of zero length and requires no orientation node. A small distance between the nodes joined by the beam is permitted. The local coordinate system which determines (r,s,t) is given by the coordinate ID in the cross sectional input, see *SECTION_BEAM, where the global system is the default. The local coordinate system axes can rotate with either node of the beam or an average rotation of both nodes . Catastrophic failure based on force resultants occurs if the following inequality is satisfied. ( 𝐹𝑟 fail 𝐹𝑟 ) + ( 𝐹𝑠 fail 𝐹𝑠 ) + ( 𝐹𝑡 fail 𝐹𝑡 ) + ( 𝑀𝑟 fail 𝑀𝑟 ) + ( 𝑀𝑠 fail 𝑀𝑠 ) + ( 𝑀𝑡 fail 𝑀𝑡 ) − 1. ≥ 0. After failure the discrete element is deleted. Likewise, catastrophic failure based on displacement resultants occurs if the following inequality is satisfied: ( 𝑢𝑟 fail 𝑢𝑟 ) + ( 𝑢𝑠 fail 𝑢𝑠 ) + ( 𝑢𝑡 fail 𝑢𝑡 ) + ( ) 𝜃𝑟 fail 𝜃𝑟 + ( 𝜃𝑠 fail 𝜃𝑠 ) + ( 𝜃𝑡 fail 𝜃𝑡 ) − 1. ≥ 0. PLASTIC DISPLACEMENT Figure M68-1. The resultant forces and moments are limited by the yield definition. The initial yield point corresponds to a plastic displacement of zero After failure the discrete element is deleted. If failure is included either one or both of the criteria may be used. *MAT_SID_DAMPER_DISCRETE_BEAM This is Material Type 69. The side impact dummy uses a damper that is not adequately treated by the nonlinear force versus relative velocity curves since the force characteristics are dependent on the displacement of the piston. See also notes below. Card 1 1 Variable MID Type A8 Card 2 Variable 1 C3 2 RO F 2 3 ST F 3 STF RHOF Type F F F 4 D F 4 C1 F 5 R F 5 C2 F 6 H F 6 7 K F 7 LCIDF LCIDD F F 8 C F 8 S0 F Orifrice Cards. Include on card per orifice. Read in up to 15 orifice locations. Input is terminated when a “*” card is found. On the first card below the optional input parameters SF and DF may be specified. Cards 3 1 2 Variable ORFLOC ORFRAD Type F F 3 SF F 4 DC F 5 6 7 8 VARIABLE MID RO ST D R DESCRIPTION Material identification. A unique number or label not exceeding 8 characters must be specified. Mass density, see also volume on *SECTION_BEAM definition. St, piston stroke. St must equal or exceed the length of the beam element, see Figure M69-1 below. d, piston diameter R, default orifice radius H K C C3 STF *MAT_SID_DAMPER_DISCRETE_BEAM DESCRIPTION h, orifice controller position K, damping constant LT.0.0: |K| is the load curve number ID, see *DEFINE_- CURVE, defining the damping coefficient as a function of the absolute value of the relative velocity. C, discharge coefficient Coefficient for fluid inertia term k, stiffness coefficient if piston bottoms out RHOF ρ𝑓𝑙𝑢𝑖𝑑, fluid density C1 C2 LCIDF LCIDD C1, coefficient for linear velocity term C2, coefficient for quadratic velocity term Load curve number ID defining force versus piston displacement, s, i.e., term 𝑓 (𝑠 + 𝑠0). Compressive behavior is defined in the positive quadrant of the force displacement curve. Displacements falling outside of the defined force displacement curve are extrapolated. Care must be taken to ensure that extrapolated values are reasonable. Load curve number ID defining damping coefficient versus piston displacement, s, i.e., 𝑔(𝑠 + 𝑠0). Displacements falling outside the defined curve are extrapolated. Care must be taken to ensure that extrapolated values are reasonable. S0 Initial displacement s0, typically set to zero. displacement corresponds to compressive behavior. A positive ORFLOC di, orifice location of ith orifice relative to the fixed end. ORFRAD ri, orifice radius of ith orifice, if zero the default radius is used. SF DC Scale factor on calculated force. The default is set to 1.0 c, linear viscous damping coefficient used after damper bottoms out either in tension or compression. Remarks: As the damper moves, the fluid flows through the open orifices to provide the necessary damping resistance. While moving as shown in Figure M69-1 the piston gradually blocks off and effectively closes the orifices. The number of orifices and the size of their opening control the damper resistance and performance. The damping force is computed from, 𝐹 = SF × {⎧ ⎩{⎨ 𝐾𝐴𝑝𝑉𝑝 {⎧𝐶1 ⎩{⎨ 𝐴0 𝑡 + 𝐶2∣𝑉𝑝∣𝜌fluid 𝐴𝑝 𝐶𝐴0 𝑡 ) ⎡( ⎢ ⎣ − 1 }⎫ ⎤ ⎥ ⎭}⎬ ⎦ }⎫ − 𝑓 (𝑠 + 𝑠0) + 𝑉𝑝𝑔(𝑠 + 𝑠0) ⎭}⎬ where K is a user defined constant or a tabulated function of the absolute value of the relative velocity, Vp is the piston velocity, C is the discharge coefficient, Ap is the piston 𝑡 is the total open areas of orifices at time t, ρfluid is the fluid density, C1 is the area, 𝐴0 coefficient for the linear term, and C2 is the coefficient for the quadratic term. d4 d3 d2 d1 Piston Vp ith Piston Orifice Orifice Opening Controller Figure M69-1. Mathematical model for the Side Impact Dummy damper. 2Ri - h In the implementation, the orifices are assumed to be circular with partial covering by the orifice controller. As the piston closes, the closure of the orifice is gradual. This gradual closure is properly taken into account to insure a smooth response. If the piston stroke is exceeded, the stiffness value, k, limits further movement, i.e., if the damper bottoms out in tension or compression the damper forces are calculated by replacing the damper by a bottoming out spring and damper, k and c, respectively. The piston stroke must exceed the initial length of the beam element. The time step calculation is based in part on the stiffness value of the bottoming out spring. A typical force versus displacement curve at constant relative velocity is shown in Figure M69-2. The factor, SF, which scales the force defaults to 1.0 and is analogous to the adjusting ring on the damper. Last orifice closes. Force increases as orifice is gradually covered. DISPLACEMENT Figure M69-2. Force versus displacement as orifices are covered at a constant relative velocity. Only the linear velocity term is active. *MAT_HYDRAULIC_GAS_DAMPER_DISCRETE_BEAM This is Material Type 70. This special purpose element represents a combined hydraulic and gas-filled damper which has a variable orifice coefficient. A schematic of the damper is shown in Figure M70-1. Dampers of this type are sometimes used on buffers at the end of railroad tracks and as aircraft undercarriage shock absorbers. This material can be used only as a discrete beam element. See also notes below. Card 1 1 Variable MID 2 RO Type A8 F Card 2 1 Variable LCID Type F 2 FR F 3 CO F 3 4 N F 4 SCLF CLEAR F F 5 P0 F 5 6 PA F 6 7 AP F 7 8 KH F 8 VARIABLE MID RO CO N P0 PA AP KH DESCRIPTION Material identification. A unique number or label not exceeding 8 characters must be specified. Mass density, see also volume in *SECTION_BEAM definition. Length of gas column, Co Adiabatic constant Initial gas pressure, P0 Atmospheric pressure, Pa Piston cross sectional area, Ap Hydraulic constant, K LCID Load curve ID, see *DEFINE_CURVE, defining the orifice area, a0, versus element deflection. Orifice VARIABLE FR Oil Profiled Pin Gas Figure M70-1. Schematic of Hydraulic/Gas damper. DESCRIPTION Return factor on orifice force. This acts as a factor on the hydraulic force only and is applied when unloading. It is intended to represent a valve that opens when the piston unloads to relieve hydraulic pressure. Set it to 1.0 for no such relief. SCLF Scale factor on force. (Default = 1.0) CLEAR Clearance (if nonzero, no tensile force develops for positive displacements and negative forces develop only after the clearance is closed. Remarks: As the damper is compressed two actions contribute to the force which develops. First, the gas is adiabatically compressed into a smaller volume. Secondly, oil is forced through an orifice. A profiled pin may occupy some of the cross-sectional area of the orifice; thus, the orifice area available for the oil varies with the stroke. The force is assumed proportional to the square of the velocity and inversely proportional to the available area. The equation for this element is: 𝐹 = SCLF × {𝐾ℎ ( 𝑎0 ) + [𝑃0 ( 𝐶0 𝐶0 − 𝑆 ) − 𝑃𝑎] 𝐴𝑝} where S is the element deflection and V is the relative velocity across the element. *MAT_071 This is Material Type 71. This model permits elastic cables to be realistically modeled; thus, no force will develop in compression. Card 1 1 Variable MID 2 RO Type A8 F 3 E F 4 LCID F Default none none none none 5 F0 F 0 6 7 8 TMAXF0 TRAMP IREAD F 0 F 0 I 0 Additional card for IREAD > 1. Card 2 1 2 3 4 5 6 7 8 Variable OUTPUT TSTART FRACL0 MXEPS MXFRC Type Default I 0 F 0 F 0 F F 1.0E+20 1.0E+20 VARIABLE DESCRIPTION MID RO E LCID F0 Material identification. A unique number or label not exceeding 8 characters must be specified. Mass density, see also volume in *SECTION_BEAM definition. GT.0.0: Young’s modulus LT.0.0: Stiffness Load curve ID, see *DEFINE_CURVE, defining the stress versus engineering strain. (Optional). Initial tensile force. If F0 is defined, an offset is not needed for an initial tensile force. TMAXF0 Time for which pre-tension force will be held *MAT_CABLE_DISCRETE_BEAM DESCRIPTION TRAMP Ramp-up time for pre-tension force IREAD Set to 1 to read second line of input OUTPUT Flag = 1 to output axial strain TSTART Time at which the ramp-up of pre-tension begins FRACL0 Fraction of initial length that should be reached over time period of TRAMP. Corresponding tensile force builds up as necessary to reach cable length = FRACL0 × L0 at time t = TRAMP. MXEPS Maximum strain at failure MXFRC Maximum force at failure Remarks: The force, F, generated by the cable is nonzero if and only if the cable is tension. The force is given by: where ΔL is the change in length 𝐹 = max(𝐹0 + 𝐾Δ𝐿, 0. ) Δ𝐿 = current length − (initial length − offset) and the stiffness (E > 0.0 only ) is defined as: 𝐾 = 𝐸 × area (initial length − offset) Note that a constant force element can be obtained by setting: although the application of such an element is unknown. 𝐹0 > 0 and 𝐾 = 0 The area and offset are defined on either the cross section or element cards. For a slack cable the offset should be input as a negative length. For an initial tensile force the offset should be positive. If a load curve is specified the Young’s modulus will be ignored and the load curve will be used instead. The points on the load curve are defined as engineering stress versus engineering strain, i.e., the change in length over the initial length. The unloading behavior follows the loading. By default, cable pretension is applied only at the start of the analysis. If the cable is attached to flexible structure, deformation of the structure will result in relaxation of the cables, which will therefore lose some or all of the intended preload. This can be overcome by using TMAXF0. In this case, it is expected that the structure will deform under the loading from the cables and that this deformation will take time to occur during the analysis. The unstressed length of the cable will be continuously adjusted until time TMAXF0 such that the force is maintained at the user-defined pre- tension force – this is analogous to operation of the pre-tensioning screws in real cables. After time TMAXF0, the unstressed length is fixed and the force in the cable is determined in the normal way using the stiffness and change of length. Sudden application of the cable forces at time zero may result in an excessively dynamic response during pre-tensioning. A ramp-up time TRAMP may optionally be defined. The cable force ramps up from zero at time TSTART to the full pre-tension F0 at time TSTART + TRAMP. TMAXF0, if set less than TSTART + TRAMP by the user, will be internally reset to TSTART + TRAMP. If the model does not use dynamic relaxation, it is recommended that damping be applied during pre-tensioning so that the structure reaches a steady state by time TMAXF0. If the model uses dynamic relaxation, TSTART, TRAMP, and TMAXF0 apply only during dynamic relaxation. The cable preload at the end of dynamic relaxation carries over to the start of the subsequent transient analysis. The cable mass will be calculated from length × area × density if VOL is set to zero on *SECTION_BEAM. Otherwise, VOL × density will be used. If OUTPUT is set to 1, one additional history variable representing axial strain is output to d3plot for the cable elements. This axial strain can be plotted by LS-PrePost by selecting the beam component labeled as “axial stress”. Though the label says “axial stress”, it is actually axial strain. If the stress-strain load curve option, LCID, is combined with preload, two types of behavior are available: 1. 2. If the preload is applied using the TMAXF0/TRAMP method, the initial strain is calculated from the stress-strain curve to achieve the desired preload. If TMAXF0/TRAMP are not used, the preload force is taken as additional to the force calculated from the stress/strain curve. Thus, the total stress in the cable will be higher than indicated by the stress/strain curve. *MAT_CONCRETE_DAMAGE This is Material Type 72. This model has been used to analyze buried steel reinforced concrete structures subjected to impulsive loadings. A newer version of this model is available as *MAT_CONCRETE_DAMAGE_REL3 4 5 6 7 8 Card 1 1 Variable MID 2 RO Type A8 F 3 PR F Default none none none 5 6 7 8 Card 2 1 Variable SIGF Type F 2 A0 F 3 A1 F 4 A2 F Default 0.0 0.0 0.0 0.0 Card 3 1 2 3 4 5 Variable A0Y A1Y A2Y A1F A2F Type F F F F F 6 B1 F 7 B2 F 8 B3 F Default 0.0 0.0 0.0 0.0 0.0 0.0 0.0 0.0 Card 4 1 Variable PER Type F 2 ER F 3 4 5 6 7 8 PRR SIGY ETAN LCP LCR F F F F F Default 0.0 0.0 0.0 none 0.0 none none Card 5 Variable Type 1 λ F 2 λ2 F 3 λ3 F 4 λ4 F 5 λ5 F 6 λ6 F 7 λ7 F 8 λ8 F Default none none none none none none none none Card 6 Variable 1 λ9 2 3 4 5 6 7 8 λ10 λ11 λ12 λ13 Type F F F F F Default none none none none none Card 7 Variable 1 η1 Type F 2 η2 F 3 η3 F 4 η4 F 5 η5 F 6 η6 F 7 η7 F 8 η8 F Default none none none none none none none none Variable 1 η9 *MAT_CONCRETE_DAMAGE 2 3 4 5 6 7 8 η10 η11 η12 η13 Type F F F F F Default none none none none none VARIABLE DESCRIPTION MID RO PR Material identification. A unique number or label not exceeding 8 characters must be specified. Mass density. Poisson’s ratio. SIGF Maximum principal stress for failure. A0 A1 A2 A0Y A1Y A2Y A1F A2F B1 B2 B3 PER ER Cohesion. Pressure hardening coefficient. Pressure hardening coefficient. Cohesion for yield Pressure hardening coefficient for yield limit Pressure hardening coefficient for yield limit Pressure hardening coefficient for failed material. Pressure hardening coefficient for failed material. Damage scaling factor. Damage scaling factor for uniaxial tensile path. Damage scaling factor for triaxial tensile path. Percent reinforcement. Elastic modulus for reinforcement. VARIABLE DESCRIPTION PRR SIGY Poisson’s ratio for reinforcement. Initial yield stress. ETAN Tangent modulus/plastic hardening modulus. Load curve ID giving rate sensitivity for principal material, see *DEFINE_CURVE. Load curve ID giving rate sensitivity for reinforcement, see *DE- FINE_CURVE. Tabulated damage function Tabulated scale factor. LCP LCR λ1 - λ13 η1 - η13 Remarks: 1. Cohesion for failed material 𝑎0𝑓 = 0. 2. B3 must be positive or zero. 3. 𝜆𝑛 ≤ 𝜆𝑛+1. The first point must be zero. *MAT_CONCRETE_DAMAGE_REL3 This is Material Type 72R3. The Karagozian & Case (K&C) Concrete Model - Release III is a three-invariant model, uses three shear failure surfaces, includes damage and strain-rate effects, and has origins based on the Pseudo-TENSOR Model (Material Type 16). The most significant user improvement provided by Release III is a model parameter generation capability, based solely on the unconfined compression strength of the concrete. The implementation of Release III significantly changed the user input, thus previous input files using Material Type 72, i.e. prior to LS-DYNA Version 971, are not compatible with the present input format. An open source reference, that precedes the parameter generation capability, is provided in Malvar et al. [1997]. A workshop proceedings reference, Malvar et al. [1996], is useful, but may be difficult to obtain. More recent, but limited distribution reference materials, e.g. Malvar et al. [2000], may be obtained by contacting Karagozian & Case. Seven card images are required to define the complete set of model parameters for the K&C Concrete Model. An Equation-of-State is also required for the pressure-volume strain response. Brief descriptions of all the input parameters are provided below, however it is expected that this model will be used primarily with the option to automatically generate the model parameters based on the unconfined compression strength of the concrete. These generated material parameters, along with the generated parameters for *EOS_TABULATED_COMPACTION, are written to the d3hsp file. 4 5 6 7 8 Card 1 1 Variable MID 2 RO Type A8 F 3 PR F Default none none none Card 2 Variable 1 FT Type F 2 A0 F 3 A1 F 4 A2 F 5 B1 F 6 7 8 OMEGA A1F F F Default none 0.0 0.0 0.0 0.0 none 0.0 Card 3 Variable 1 Sλ 2 3 4 5 6 7 8 NOUT EDROP RSIZE UCF LCRATE LOCWID NPTS Type F F F F F I F F Default none none none none none none none none Card 4 1 2 3 4 5 6 7 8 Variable λ01 λ02 λ03 λ04 λ05 λ06 λ07 λ08 Type F F F F F F F F Default none none none none none none none none Card 5 1 2 3 4 5 Variable λ09 λ10 λ11 λ12 λ13 Type F F F F F 6 B3 F 7 8 A0Y A1Y F F Default none none none none none none 0.0 0.0 Card 6 1 2 3 4 5 6 7 8 Variable η01 η02 η03 η04 η05 η06 η07 η08 Type F F F F F F F F Default none none none none none none none none Card 7 1 2 3 4 5 Variable η09 η10 η11 η12 η13 Type F F F F F 6 B2 F 7 8 A2F A2Y F F Default none none none none none 0.0 0.0 0.0 VARIABLE MID DESCRIPTION Material identification. A unique number or label not exceeding 8 characters must be specified. RO PR FT A0 A1 A2 B1 Mass density. Poisson’s ratio, 𝜈. Uniaxial tensile strength, 𝑓𝑡. Maximum shear failure surface parameter, 𝑎0 or −𝑓𝑐 parameter generation (recommended). ′ for Maximum shear failure surface parameter, 𝑎1. Maximum shear failure surface parameter, 𝑎2. Compressive damage scaling parameter, 𝑏1 OMEGA Fractional dilatancy, 𝜔. A1F Sλ 2-392 (EOS) Residual failure surface coefficient, 𝑎1𝑓 . VARIABLE DESCRIPTION NOUT Output selector for effective plastic strain . EDROP RSIZE UCF LCRATE LOCWID NPTS λ01 λ02 λ03 λ04 λ05 λ06 λ07 λ08 λ09 λ10 λ11 λ12 Post peak dilatancy decay, 𝑁𝛼. Unit conversion factor for length (inches/user-unit), e.g. 39.37 if user length unit in meters. Unit conversion factor for stress (psi/user-unit), e.g. 145 if 𝑓′𝑐 in MPa. Define (load) curve number for strain-rate effects; effective strain rate on abscissa (negative = tension) and strength enhancement on ordinate. If LCRATE is set to -1, strain rate effects are automatically included, based on equations provided in Wu, Crawford, Lan, and Magallanes [2014]. Three times the maximum aggregate diameter (input in user length units). Number of points in 𝜆 versus 𝜂 damage relation; must be 13 points. 1st value of damage function, (a.k.a., 1st value of “modified” effective plastic strain; see references for details). 2nd value of damage function, 3rd value of damage function, 4th value of damage function, 5th value of damage function, 6th value of damage function, 7th value of damage function, 8th value of damage function, 9th value of damage function, 10th value of damage function, 11th value of damage function, 12th value of damage function, VARIABLE DESCRIPTION λ13 B3 A0Y A1Y η01 η02 η03 η04 η05 η06 η07 η08 η09 η10 η11 η12 η13 B2 A2F A2Y 13th value of damage function. Damage scaling coefficient for triaxial tension, 𝑏3. Initial yield surface cohesion, 𝑎0𝑦. Initial yield surface coefficient, 𝑎1𝑦. 1st value of scale factor, 2nd value of scale factor, 3rd value of scale factor, 4th value of scale factor, 5th value of scale factor, 6th value of scale factor, 7th value of scale factor, 8th value of scale factor, 9th value of scale factor, 10th value of scale factor, 11th value of scale factor, 12th value of scale factor, 13th value of scale factor. Tensile damage scaling exponent, 𝑏2. Residual failure surface coefficient, 𝑎2𝑓 . Initial yield surface coefficient, 𝑎2𝑦. λ, sometimes referred to as “modified” effective plastic strain, is computed internally as a function of effective plastic strain, strain rate enhancement factor, and pressure. η is a function of λ as specified by the η vs. λ curve. The η value, which is always between 0 and 1, is used to interpolate between the yield failure surface and the maximum failure surface, or between the maximum failure surface and the residual failure surface, depending on whether λ is to the left or right of the first peak in the the η vs. λ curve. The “scaled damage measure” ranges from 0 to 1 as the material transitions from the yield failure surface to the maximum failure surface, and thereafter ranges from 1 to 2 as the material ranges from the maximum failure surface to the residual failure surface. See the references for details. Output of Selected Variables: The quantity labeled as “plastic strain” by LS-PrePost is actually the quantity described in Table M72-1, in accordance with the input value of NOUT . NOUT Function Description 1 2 3 4 Current shear failure surface radius 𝛿 = 2𝜆/(𝜆 + 𝜆𝑚) 𝜎̇𝑖𝑗𝜀̇𝑖𝑗 𝑝 𝜎̇𝑖𝑗𝜀̇𝑖𝑗 Scaled damage measure Strain energy (rate) Plastic strain energy (rate) Table M72-1. Description of quantity labeled “plastic strain” by LS-PrePost. An additional six extra history variables as shown in Table M72-2 may be be written by setting NEIPH = 6 on the keyword *DATABASE_EXTENT_BINARY. The extra history variables are labeled as "history var#1" through "history var#6" in LS-PrePost. Label Description history var#1 Internal energy history var#2 Pressure from bulk viscosity history var#3 Volume in previous time step history var#4 history var#5 history var#6 Plastic volumetric strain Slope of damage evolution (η vs. λ) curve “Modified” effective plastic strain (λ) Table M72-2. Extra History Variables for *MAT_072R3 Sample Input for Concrete: As an example of the K&C Concrete Model material parameter generation, the following sample input for a 45.4 MPa (6,580 psi) unconfined compression strength concrete is provided. The basic units for the provided parameters are length in millimeters (mm), time in milliseconds (msec), and mass in grams (g). This base unit set yields units of force in Newtons (N) and pressure in Mega-Pascals (MPa). Card 1 1 Variable MID 2 RO Type 72 2.3E-3 Card 2 Variable 1 FT 2 A0 Type -45.4 3 PR 3 A1 4 5 6 7 8 4 A2 5 B1 6 7 8 OMEGA A1F Card 3 Variable 1 Sλ 2 3 4 5 6 7 8 NOUT EDROP RSIZE UCF LCRATE LOCWID NPTS Type 3.94E-2 145.0 723.0 Card 4 1 2 3 4 5 6 7 8 Variable λ01 λ02 λ03 λ04 λ05 λ06 λ07 λ08 Type Card 5 1 2 3 4 5 Variable λ09 λ10 λ11 λ12 λ13 6 B3 7 8 A0Y A1Y Type Card 6 1 2 3 4 5 6 7 8 Variable η01 η02 η03 η04 η05 η06 η07 η08 Type Card 7 1 2 3 4 5 Variable η09 η10 η11 η12 η13 6 B2 7 8 A2F A2Y Type Shear strength enhancement factor versus effective strain rate is given by a curve (*DE- FINE_CURVE) with LCID 723. The sample input values, see Malvar & Ross [1998], are given in Table M72-3. Strain-Rate (1/ms) Enhancement -3.0E+01 -3.0E-01 -1.0E-01 -3.0E-02 -1.0E-02 -3.0E-03 -1.0E-03 -1.0E-04 -1.0E-05 -1.0E-06 -1.0E-07 -1.0E-08 0.0E+00 3.0E-08 1.0E-07 1.0E-06 1.0E-05 1.0E-04 1.0E-03 3.0E-03 1.0E-02 3.0E-02 1.0E-01 3.0E-01 3.0E+01 9.70 9.70 6.72 4.50 3.12 2.09 1.45 1.36 1.28 1.20 1.13 1.06 1.00 1.00 1.03 1.08 1.14 1.20 1.26 1.29 1.33 1.36 2.04 2.94 2.94 Table M72-3. Enhancement versus effective strain rate for 45.4 MPa concrete (sample). When defining curve LCRATE, input negative (tensile) values of effective strain rate first. The enhancement should be positive and should be 1.0 at a strain rate of zero. *MAT_LOW_DENSITY_VISCOUS_FOAM This is Material Type 73 for Modeling Low Density Urethane Foam with high compressibility and with rate sensitivity which can be characterized by a relaxation curve. Its main applications are for seat cushions, padding on the Side Impact Dummies (SID), bumpers, and interior foams. Optionally, a tension cut-off failure can be defined. Also, see the notes below and the description of material 57: *MAT_LOW_- DENSITY_FOAM. Card 1 1 Variable MID 2 RO Type A8 F 3 E F 4 LCID F 5 TC F 6 HU F 7 8 BETA DAMP F F Default Remarks 1.E+20 1. 0.05 3 6 1 7 8 Card 2 1 2 3 4 5 Variable SHAPE FAIL BVFLAG KCON LCID2 BSTART TRAMP NV Type F F F F Default 1.0 0.0 0.0 0.0 F 0 F F 0.0 0.0 I 6 Relaxation Constant Cards. If LCID2 = 0 then include the following viscoelastic constants. Up to 6 cards may be input. A keyword card (with a “*” in column 1) terminates this input if less than 6 cards are used. Card 3 Variable Type 1 GI F 2 3 4 5 6 7 8 BETAI REF F Frequency Dependence Card. If LCID2 = -1 then include the following frequency dependent viscoelastic data. Card 4 1 2 3 4 5 6 7 8 Variable LCID3 LCID4 SCALEW SCALEA Type I I I I VARIABLE DESCRIPTION MID RO E LCID TC HU Material identification. A unique number or label not exceeding 8 characters must be specified. Mass density Young’s modulus used in tension. For implicit problems E is set to the initial slope of load curve LCID. Load curve ID, see *DEFINE_CURVE, for nominal stress versus strain. Tension cut-off stress Hysteretic unloading factor between 0 and 1 (default = 1, i.e., no energy dissipation), see also Figure M57-1 BETA β, decay constant to model creep in unloading. EQ.0.0: No relaxation. DAMP Viscous coefficient (.05 < recommended value <.50) to model damping effects. LT.0.0: |DAMP| is the load curve ID, which defines the damping constant as a function of the maximum strain in compression defined as: 𝜀max = max(1 − 𝜆1, 1 − 𝜆2, 1. −𝜆3) In tension, the damping constant is set to the value corre- sponding to the strain at 0. The abscissa should be defined from 0 to 1. SHAPE Shape factor for unloading. Active for nonzero values of the hysteretic unloading factor. Values less than one reduces the energy dissipation and greater than one increases dissipation, see also Figure M57-1. VARIABLE DESCRIPTION FAIL Failure option after cutoff stress is reached: EQ.0.0: tensile stress remains at cut-off value, EQ.1.0: tensile stress is reset to zero. BVFLAG Bulk viscosity activation flag, see remark below: EQ.0.0: no bulk viscosity (recommended), EQ.1.0: bulk viscosity active. KCON LCID2 BSTART Stiffness coefficient for contact interface stiffness. Maximum slope in stress vs. strain curve is used. When the maximum slope is taken for the contact, the time step size for this material is reduced for stability. In some cases Δt may be significantly smaller, and defining a reasonable stiffness is recommended. Load curve ID of relaxation curve. If constants 𝛽𝑡 are determined via a least squares fit. This relaxation curve is shown in Figure M76-1. This model ignores the constant stress. Fit parameter. In the fit, 𝛽1 is set to zero, 𝛽2 is set to BSTART, 𝛽3 is 10 times 𝛽2, 𝛽4 is 10 times greater than 𝛽3 , and so on. If zero, BSTART = .01. TRAMP Optional ramp time for loading. NV Number of terms in fit. If zero, the default is 6. Currently, the maximum number is set to 6. Values of 2 are 3 are recommended, since each term used adds significantly to the cost. Caution should be exercised when taking the results from the fit. Preferably, all generated coefficients should be positive. Negative values may lead to unstable results. Once a satisfactory fit has been achieved it is recommended that the coefficients which are written into the output file be input in future runs. Gi Optional shear relaxation modulus for the ith term BETAi Optional decay constant if ith term REF *MAT_LOW_DENSITY_VISCOUS_FOAM DESCRIPTION Use reference geometry to initialize the stress tensor. The reference geometry is defined by the keyword:*INITIAL_FOAM_- REFERENCE_GEOMETRY . EQ.0.0: off, EQ.1.0: on. LCID3 LCID4 Load curve ID giving the magnitude of the shear modulus as a function of the frequency. LCID3 must use the same frequencies as LCID4. Load curve ID giving the phase angle of the shear modulus as a function of the frequency. LCID4 must use the same frequencies as LCID3. SCALEW Flag for the form of the frequency data. EQ.0.0: Frequency is in cycles per unit time. EQ.1.0: Circular frequency. SCALEA Flag for the units of the phase angle. EQ.0.0: Degrees. EQ.1.0: Radians. Material Formulation: This viscoelastic foam model is available to model highly compressible viscous foams. The hyperelastic formulation of this model follows that of Material 57. Rate effects are accounted for through linear viscoelasticity by a convolution integral of the form 𝜎𝑖𝑗 𝑟 = ∫ 𝑔𝑖𝑗𝑘𝑙(𝑡 − 𝜏) ∂𝜀𝑘𝑙 ∂𝜏 𝑑𝜏 where 𝑔𝑖𝑗𝑘𝑙(𝑡 − 𝜏) is the relaxation function. The stress tensor, 𝜎𝑖𝑗 determined from the foam, 𝜎𝑖𝑗 summation of the two contributions: 𝑟 , augments the stresses 𝑓 ; consequently, the final stress, 𝜎𝑖𝑗, is taken as the 𝜎𝑖𝑗 = 𝜎𝑖𝑗 𝑓 + 𝜎𝑖𝑗 𝑟 . Since we wish to include only simple rate effects, the relaxation function is represented by up to six terms of the Prony series: 𝑔(𝑡) = 𝛼0 + ∑ 𝛼𝑚𝑒−𝛽𝑚𝑡 𝑚=1 This model is effectively a Maxwell fluid which consists of a dampers and springs in series. The formulation is performed in the local system of principal stretches where only the principal values of stress are computed and triaxial coupling is avoided. Consequently, the one-dimensional nature of this foam material is unaffected by this addition of rate effects. The addition of rate effects necessitates 42 additional history variables per integration point. The cost and memory overhead of this model comes primarily from the need to “remember” the local system of principal stretches and the evaluation of the viscous stress components. Frequency data can be fit to the Prony series. Using Fourier transforms the relationship between the relaxation function and the frequency dependent data is 𝐺𝑠(𝜔) = 𝛼0 + ∑ 𝑚=1 𝛼𝑚(𝜔/𝛽𝑚)2 1 + (𝜔/𝛽𝑚)2 𝐺ℓ(𝜔) = ∑ 𝑚=1 𝛼𝑚𝜔/𝛽𝑚 1 + 𝜔/𝛽𝑚 where the storage modulus and loss modulus are defined in terms of the frequency dependent magnitude G and phase angle 𝜙 given by load curves LCID3 and LCID4 respectively, 𝐺𝑠(𝜔) = 𝐺(𝜔) cos[𝜙(𝜔)] , and 𝐺𝑙(𝜔) = 𝐺(𝜔) sin[𝜙(𝜔)] Remarks: When hysteretic unloading is used the reloading will follow the unloading curve if the decay constant, β, is set to zero. If β is nonzero the decay to the original loading curve is governed by the expression: 1 − 𝑒−𝛽𝑡 The bulk viscosity, which generates a rate dependent pressure, may cause an unexpected volumetric response and, consequently, it is optional with this model. The hysteretic unloading factor results in the unloading curve to lie beneath the loading curve as shown in Figure M57-1. This unloading provides energy dissipation which is reasonable in certain kinds of foam. *MAT_ELASTIC_SPRING_DISCRETE_BEAM This is Material Type 74. This model permits elastic springs with damping to be combined and represented with a discrete beam element type 6. Linear stiffness and damping coefficients can be defined, and, for nonlinear behavior, a force versus deflection and force versus rate curves can be used. Displacement based failure and an initial force are optional. Card 1 1 Variable MID Type A8 Card 2 1 2 RO F 2 Variable FLCID HLCID Type F F 3 K F 3 C1 F 4 F0 F 4 C2 F 5 D F 5 6 7 8 CDF TDF F 6 F 7 8 DLE GLCID F I VARIABLE DESCRIPTION MID RO K F0 D CDF TDF Material identification. A unique number or label not exceeding 8 characters must be specified. Mass density, see also volume in *SECTION_BEAM definition. Stiffness coefficient. Optional initial force. This option is inactive if this material is referenced in a part referenced by material type *MAT_ELAS- TIC_6DOF_SPRING Viscous damping coefficient. Compressive displacement at failure. Input as a positive number. After failure, no forces are carried. This option does not apply to zero length springs. EQ.0.0: inactive. Tensile displacement at failure. After failure, no forces are carried. VARIABLE DESCRIPTION FLCID HLCID C1 C2 Load curve ID, see *DEFINE_CURVE, defining force versus deflection for nonlinear behavior. Load curve ID, see *DEFINE_CURVE, defining force versus relative velocity for nonlinear behavior (optional). If the origin of the curve is at (0,0) the force magnitude is identical for a given magnitude of the relative velocity, i.e., only the sign changes. Damping coefficient for nonlinear behavior (optional). Damping coefficient for nonlinear behavior (optional). DLE Factor to scale time units. The default is unity. GLCID Optional load curve ID, see *DEFINE_CURVE, defining a scale factor versus deflection for load curve ID, HLCID. If zero, a scale factor of unity is assumed. Remarks: If the linear spring stiffness is used, the force, F, is given by: 𝐹 = 𝐹0 + KΔ𝐿 + DΔ𝐿̇ but if the load curve ID is specified, the force is then given by: 𝐹 = 𝐹0 + K𝑓 (Δ𝐿) {1 + C1 × Δ𝐿̇ + C2 × sgn(Δ𝐿̇)ln [max (1. , Δ𝐿̇ DLE )]} + DΔ𝐿̇ + 𝑔(Δ𝐿)ℎ(Δ𝐿̇) In these equations, Δ𝐿 is the change in length Δ𝐿 = current length − initial length The cross sectional area is defined on the section card for the discrete beam elements, See *SECTION_BEAM. The square root of this area is used as the contact thickness offset if these elements are included in the contact treatment. *MAT_BILKHU/DUBOIS_FOAM This is Material Type 75. This model is for the simulation of isotropic crushable foams. Uniaxial and triaxial test data are used to describe the behavior. Card 1 1 Variable MID Type A8 Card 2 1 2 RO F 2 3 4 5 YM LCPY LCUYS F 3 F 4 F 5 6 VC F 6 7 PC F 8 VPC F 7 8 Variable TSC VTSC LCRATE PR KCON ISFLG NCYCLE Type I F F F F F F VARIABLE DESCRIPTION MID RO YM LCPY LCUYS VC PC Material identification. A unique number or label not exceeding 8 characters must be specified. Mass density Young’s modulus 𝐸 Load curve ID giving pressure for plastic yielding versus volumetric strain, see Figure M75-1. Load curve ID giving uniaxial yield stress versus volumetric strain, see Figure M75-1, all abscissa values should be positive if only the results of a compression test are included, optionally the results of a tensile test can be added (corresponding to negative values of the volumetric strain), in the latter case PC, VPC, TC and VTC will be ignored Viscous damping coefficient (0.05 < recommended value < 0.50; default is 0.05). Pressure cutoff for hydrostatic tension. If zero, the default is set to one-tenth of 𝑝0, the yield pressure corresponding to a volumetric strain of zero. PC will be ignored if TC is non zero. True Stress optional Uniaxial Yield Stress (LCUYS) Pressure Yield (LCPY) tension compression Volumetric Strain Figure M75-1. Behavior of crushable foam. Unloading is elastic. VARIABLE DESCRIPTION VPC TC VTC Variable pressure cutoff for hydrostatic tension as a fraction of pressure yield value. If non-zero this will override the pressure cutoff value PC. Tension cutoff for uniaxial tensile stress. Default is zero. A nonzero value is recommended for better stability. Variable tension cutoff for uniaxial tensile stress as a fraction of the uniaxial compressive yield strength, if non-zero this will override the tension cutoff value TC. LCRATE Load curve ID giving a scale factor for the previous yield curves, dependent upon the volumetric strain rate. PR KCON Poisson coefficient, which applies to both elastic and plastic deformations, must be smaller then 0.5 Stiffness coefficient for contact interface stiffness. If undefined one-third of Young’s modulus, YM, is used. KCON is also considered in the element time step calculation; therefore, large values may reduce the element time step size. ISFLG *MAT_BILKHU/DUBOIS_FOAM DESCRIPTION Flag for tensile response (active only if negative abscissa are present in load curve LCUYS) EQ.0: load curve abscissa in tensile region correspond to volumetric strain EQ.1: load curve abscissa in tensile region correspond to effective strain (for large PR, when volumetric strain vanishes) NCYCLE Number of cycles to determine the average volumetric strain rate. NCYCLE is 1 by default (no smoothing) and cannot exceed 100. Remarks: The logarithmic volumetric strain is defined in terms of the relative volume, 𝑉, as: If option ISFLG = 1 is used, the effective strain is defined in the usual way: 𝛾 = −ln(𝑉) 𝜀eff = √ tr(𝛆t𝛆) In defining the load curve LCPY the stress and strain pairs should be positive values starting with a volumetric strain value of zero. The load curve LCUYS can optionally contain the results of the tensile test (correspond- ing to negative values of the volumetric strain), if so, then the load curve information will override PC, VPC, TC and VTC. The yield surface is defined as an ellipse in the equivalent pressure and von Mises stress plane. This ellipse is characterized by three points: 1. 2. 3. the hydrostatic compression limit (LCPY), the uniaxial compression limit (LCUYS), and either the pressure cutoff for hydrostatic stress (PC,VPC), the tension cutoff for uniaxial tension (TC,VTC), or the optional tensile part of LCUYS. To prevent high frequency oscillations in the strain rate from causing similar high frequency oscillations in the yield stress, a modified volumetric strain rate is used obtain the scaled yield stress. The modified strain rate is obtained as follows. If NYCLE is > 1, then the modified strain rate is obtained by a time average of the actual strain rate over NCYCLE solution cycles. The averaged strain rate is stored on history variable #3. *MAT_GENERAL_VISCOELASTIC_{OPTION} The available options include: <BLANK> MOISTURE This is Material Type 76. This material model provides a general viscoelastic Maxwell model having up to 18 terms in the Prony series expansion and is useful for modeling dense continuum rubbers and solid explosives. Either the coefficients of the Prony series expansion or a relaxation curve may be specified to define the viscoelastic deviatoric and bulk behavior. The material model can also be used with laminated shell. Either an elastic or viscoelastic layer can be defined with the laminated formulation. To activate laminated shell you need the laminated formulation flag on *CONTROL_SHELL. With the laminated option a user defined integration rule is needed. Card 1 1 Variable MID 2 RO 3 4 BULK PCF Type A8 F F F 5 EF F 6 TREF F 7 A F 8 B F Relaxation Curve Card. Leave blank if the Prony Series Cards are used below. Also, leave blank if an elastic layer is defined in a laminated shell. Card 2 1 2 3 4 5 6 7 8 Variable LCID NT BSTART TRAMP LCIDK NTK BSTARTK TRAMPK Type F I F F F I F F Moisture Card. Additional card for MOISTURE keyword option. Card 3 1 2 3 4 5 6 7 8 Variable MO ALPHA BETA GAMMA MST Type F F F F Prony Series cards. Card Format for viscoelastic constants. Up to 18 cards may be input. A keyword card (with a “*” in column 1) terminates this input if less than 18 cards are used. These cards are not needed if relaxation data is defined. The number of terms for the shear behavior may differ from that for the bulk behavior: insert zero if a term is not included. If an elastic layer is defined you only need to define GI and KI (note in an elastic layer only one card is needed) Card 4 Variable Type 1 GI F 2 BETAI F 3 KI F VARIABLE MID 4 5 6 7 8 BETAKI F DESCRIPTION Material identification. A unique number or label not exceeding 8 characters must be specified. RO Mass density. BULK Elastic bulk modulus. PCF EF TREF A B LCID NT Tensile pressure elimination flag for solid elements only. If set to unity tensile pressures are set to zero. Elastic flag (if equal 1, the layer is elastic. If 0 the layer is viscoelastic). Reference temperature for shift function (must be greater than zero). Coefficient for the Arrhenius and the Williams-Landau-Ferry shift functions. Coefficient for the Williams-Landel-Ferry shift function. Load curve ID for deviatoric relaxation behavior. If LCID is given, constants 𝐺𝑖, and 𝛽𝑖 are determined via a least squares fit. See Figure M76-1 for an example relaxation curve. Number of terms in shear fit. If zero the default is 6. Fewer than NT terms will be used if the fit produces one or more negative shear moduli. Currently, the maximum number is set to 18. σ∕ε TRAMP 10n 10n+1 10n+2 10n+3 time optional ramp time for loading Figure M76-1. Relaxation curves for deviatoric behavior and bulk behavior. The ordinate of LCID is the deviatoric stress divided by (2 times the constant value of deviatoric strain) where the stress and strain are in the direction of the prescribed strain, or in non-directional terms, the effective stress divided by (3 times the effective strain). LCIDK defines the mean stress divided by the constant value of volumetric strain imposed in a hydrostatic stress relaxation experiment, versus time. For best results, the points defined in the curve should be equally spaced on the logarithmic scale. Note the values for the abscissa are input as time, not log(time). Furthermore, the curve should be smooth and defined in the positive quadrant. If nonphysical values are determined by least squares fit, LS-DYNA will terminate with an error message after the initialization phase is completed. If the ramp time for loading is included, then the relaxation which occurs during the loading phase is taken into account. This effect may or may not be important. VARIABLE BSTART DESCRIPTION In the fit, 𝛽1 is set to zero, 𝛽2 is set to BSTART, 𝛽3 is 10 times 𝛽2, 𝛽4 is 10 times 𝛽3, and so on. If zero, BSTART is determined by an iterative trial and error scheme. TRAMP Optional ramp time for loading. LCIDK Load curve ID for bulk relaxation behavior. If LCIDK is given, constants 𝐾𝑖, and 𝛽𝑘𝑖 are determined via a least squares fit. See Figure M76-1 for an example relaxation curve. VARIABLE NTK BSTARTK DESCRIPTION Number of terms desired in bulk fit. If zero the default is 6. Currently, the maximum number is set to 18. In the fit, 𝛽𝑘1, is set to zero, 𝛽𝑘2 is set to BSTARTK, 𝛽𝑘3 is 10 times 𝛽𝑘2, 𝛽𝑘4 is 100 times greater than 𝛽𝑘3, and so on. If zero, BSTARTK is determined by an iterative trial and error scheme. TRAMPK Optional ramp time for bulk loading. MO Initial moisture, 𝑀0. Defaults to zero. ALPHA Specifies 𝛼 as a function of moisture. GT.0.0: Specifies a curve ID. LT.0.0: Specifies the negative of a constant value. BETA Specifies 𝛽 as a function of moisture. GT.0.0: Specifies a curve ID. LT.0.0: Specifies the negative of a constant value. GAMMA Specifies 𝛾 as a function of moisture. GT.0.0: Specifies a curve ID. LT.0.0: Specifies the negative of a constant value. MST Moisture, 𝑀. If the moisture is 0.0, the moisture option is disabled. GT.0.0: Specifies a curve ID to make moisture a function of time. LT.0.0: Specifies the negative of a constant value of moisture. GI Optional shear relaxation modulus for the ith term BETAI Optional shear decay constant for the ith term KI Optional bulk relaxation modulus for the ith term BETAKI Optional bulk decay constant for the ith term *MAT_GENERAL_VISCOELASTIC Rate effects are taken into accounted through linear viscoelasticity by a convolution integral of the form: 𝜎𝑖𝑗 = ∫ 𝑔𝑖𝑗𝑘𝑙(𝑡 − 𝜏) ∂𝜀𝑘𝑙 ∂𝜏 𝑑𝜏 where 𝑔𝑖𝑗𝑘𝑙(𝑡−𝜏) is the relaxation functions for the different stress measures. This stress is added to the stress tensor determined from the strain energy functional. If we wish to include only simple rate effects, the relaxation function is represented by 18 terms from the Prony series: 𝑔(𝑡) = ∑ 𝐺𝑚𝑒−𝛽𝑚𝑡 𝑚=1 We characterize this in the input by shear moduli, 𝐺𝑖, and decay constants, 𝛽𝑖. An arbitrary number of terms, up to 18, may be used when applying the viscoelastic model. For volumetric relaxation, the relaxation function is also represented by the Prony series in terms of bulk moduli: 𝑘(𝑡) = ∑ 𝐾𝑚𝑒−𝛽𝑘𝑚𝑡 𝑚=1 The Arrhenius and Williams-Landau-Ferry (WLF) shift functions account for the effects of the temperature on the stress relaxation. A scaled time, t’, 𝑡′ = ∫ Φ(𝑇)𝑑𝑡 is used in the relaxation function instead of the physical time. The Arrhenius shift function is Φ(𝑇) = exp [−𝐴 ( − 𝑇REF )] and the Williams-Landau-Ferry shift function is Φ(𝑇) = exp (−𝐴 𝑇 − 𝑇REF 𝐵 + 𝑇 − 𝑇REF ) If all three values (TREF, A, and B) are not zero, the WLF function is used; the Arrhenius function is used if B is zero; and no scaling is applied if all three values are zero. The moisture model allows the scaling of the material properties as a function of the moisture content of the material. The shear and bulk moduli are scaled by 𝛼, the decay constants are scaled by β, and a moisture strain, 𝛾(𝑀)[𝑀 − 𝑀𝑂] is introduced analogous to the thermal strain. *MAT_HYPERELASTIC_RUBBER This is Material Type 77. This material model provides a general hyperelastic rubber model combined optionally with linear viscoelasticity as outlined by Christensen [1980]. Card 1 1 Variable MID 2 RO Type A8 F 3 PR F 4 N I 5 NV I 6 G F 7 8 SIGF REF F F Hysteresis Card. Additional card read in when PR < 0 (Mullins Effect). Card 2 1 2 3 4 5 6 7 8 Variable TBHYS Type F Card 3 for N > 0. For N > 0 a least squares fit is computed from uniaxial data. Card 3 1 Variable SGL 2 SW Type F F 3 ST F 4 5 6 7 8 LCID1 DATA LCID2 BSTART TRAMP F F F F F Card 3 for N = 0. Set the material parameters directly. Card 3 1 2 3 4 5 6 7 8 Variable C10 C01 C11 C20 C02 C30 THERML Type F F F F F F Optional Viscoelastic Constants & Frictional Damping Constant Cards. Up to 12 cards may be input. A keyword card (with a “*” in column 1) terminates this input if less than 12 cards are used. Card 4 Variable Type 1 Gi F 2 BETAi F 3 Gj F 4 5 6 7 8 SIGFj F VARIABLE DESCRIPTION MID RO PR Material identification. A unique number or label not exceeding 8 characters must be specified. Mass density Poisson’s ratio (> .49 is recommended, smaller values may not work and should not be used). If this is set to a negative number, then the absolute value is used and an extra card is read for Mullins effect. TBHYS Table ID for hysteresis, could be positive or negative, see Remarks 1 and 2. N Number of constants to solve for: EQ.1: Solve for C10 and C01 EQ.2: Solve for C10, C01, C11, C20, and C02 EQ.3: Solve for C10, C01, C11, C20, C02, and C30 NV Number of Prony series terms in fit. If zero, the default is 6. Currently, the maximum number is set to 12. Values less than 12, possibly 3 - 5 are recommended, since each term used adds significantly to the cost. Caution should be exercised when taking the results from the fit. Preferably, all generated coefficients should be positive. Negative values may lead to unstable results. Once a satisfactory fit has been achieved it is recommended that the coefficients which are written into the output file be input in future runs. VARIABLE DESCRIPTION G SIGF REF Shear modulus for frequency independent damping. Frequency independent damping is based of a spring and slider in series. The critical stress for the slider mechanism is SIGF defined below. For the best results, the value of G should be 250 - 1000 times greater than SIGF. Limit stress for frequency independent frictional damping. Use reference geometry to initialize the stress tensor. The reference geometry is defined by the keyword:*INITIAL_FOAM_- REFERENCE_GEOMETRY . EQ.0.0: off, EQ.1.0: on. If N>0 test information from a uniaxial test are used. SGL SW ST LCID1 Specimen gauge length Specimen width Specimen thickness Load curve ID giving the force versus actual change in the gauge length. If SGL, SW, and ST are set to unity (1.0), then curve LCID1 is also engineering stress versus engineering strain. DATA Type of experimental data. EQ.0.0: uniaxial data (Only option for this model) LCID2 Load curve ID of the deviatoric stress relaxation curve, neglecting the long term deviatoric stress. If LCID2 is given, constants 𝐺𝑖 and 𝛽𝑖 are determined via a least squares fit. See M76-1 for an example relaxation curve. The ordinate of the curve is the viscoelastic deviatoric stress divided by (2 times the constant value of deviatoric strain) where the stress and strain are in the direction of the prescribed strain, or in non-directional terms, the effective stress divided by (3 times the effective strain). BSTART In the fit, 𝛽1 is set to zero, 𝛽2 is set to BSTART, 𝛽3 is 10 times 𝛽2, 𝛽4 is 10 times 𝛽3, and so on. If zero, BSTART is determined by an iterative trial and error scheme. TRAMP Optional ramp time for loading. VARIABLE DESCRIPTION If N=0, the following constants have to be defined: C10 C01 C11 C20 C02 C30 𝐶10 𝐶01 𝐶11 𝐶20 𝐶02 𝐶30 THERML Flag for the thermal option. If THERML > 0.0, then G, SIGF, C10 and C01 specify curve IDs giving the values as functions of temperature, otherwise they specify the constants. This option is available only for solid elements. Gi Optional shear relaxation modulus for the ith term BETAi Optional decay constant if ith term Gj SIGFj Optional shear modulus for frequency independent damping represented as the jth spring and slider in series in parallel to the rest of the stress contributions. Limit stress for frequency independent, frictional, damping represented as the jth spring and slider in series in parallel to the rest of the stress contributions. Background: Rubber is generally considered to be fully incompressible since the bulk modulus greatly exceeds the shear modulus in magnitude. To model the rubber as an unconstrained material a hydrostatic work term, 𝑊𝐻(𝐽), is included in the strain energy functional which is function of the relative volume, 𝐽, [Ogden 1984]: 𝑊(𝐽1, 𝐽2, 𝐽) = ∑ 𝐶𝑝𝑞(𝐽1 − 3)𝑝(𝐽2 − 3)𝑞 + 𝑊𝐻(𝐽) 𝑝,𝑞=0 −1 𝐽1 = 𝐼1𝐼3 −2 𝐽2 = 𝐼2𝐼3 3⁄ 3⁄ In order to prevent volumetric work from contributing to the hydrostatic work the first and second invariants are modified as shown. This procedure is described in more detail by Sussman and Bathe [1987]. Rate effects are taken into account through linear viscoelasticity by a convolution integral of the form: 𝜎𝑖𝑗 = ∫ 𝑔𝑖𝑗𝑘𝑙(𝑡 − 𝜏) ∂𝜀𝑘𝑙 ∂𝜏 𝑑𝜏 or in terms of the second Piola-Kirchhoff stress, 𝑆𝑖𝑗, and Green's strain tensor, 𝐸𝑖𝑗, 𝑆𝑖𝑗 = ∫ 𝐺𝑖𝑗𝑘𝑙(𝑡 − 𝜏) ∂𝐸𝑘𝑙 ∂𝜏 𝑑𝜏 where 𝑔𝑖𝑗𝑘𝑙(𝑡 − 𝜏) and 𝐺𝑖𝑗𝑘𝑙(𝑡 − 𝜏) are the relaxation functions for the different stress measures. This stress is added to the stress tensor determined from the strain energy functional. If we wish to include only simple rate effects, the relaxation function is represented by six terms from the Prony series: given by, 𝑔(𝑡) = 𝛼0 + ∑ 𝛼𝑚𝑒−𝛽𝑡 𝑚=1 𝑔(𝑡) = ∑ 𝐺𝑖𝑒−𝛽𝑖𝑡 𝑖=1 This model is effectively a Maxwell fluid which consists of a dampers and springs in series. We characterize this in the input by shear moduli, 𝐺𝑖, and decay constants, 𝛽𝑖. The viscoelastic behavior is optional and an arbitrary number of terms may be used. In order to avoid a constant shear modulus from this visco-elastic formulation, a term in the series is included only when 𝛽𝑖 > 0. The Mooney-Rivlin rubber model (model 27) is obtained by specifying 𝑛 = 1. In spite of the differences in formulations with model 27, we find that the results obtained with this model are nearly identical with those of material 27 as long as large values of Poisson’s ratio are used. The frequency independent damping is obtained by the having a spring and slider in series as shown in the following sketch: friction Several springs and sliders in series can be defined that are put in parallel to the rest of the stress contributions of this material model. *MAT_HYPERELASTIC_RUBBER 1. Hysteresis (TBHYS > 0). If a positive table ID for hysteresis is defined, then TBHYS is a table having curves that are functions of strain-energy density. Let 𝑊dev be the current value of the deviatoric strain energy density as calculated above. Furthermore, let 𝑊̅̅̅̅̅̅dev be the peak strain energy density reached up to this point in time. It is then assumed that the resulting stress is reduced by a damage factor according to 𝐒 = 𝐷(𝑊dev, 𝑊̅̅̅̅̅̅dev) ∂𝑊dev ∂𝐄 + ∂𝑊vol ∂𝐄 . where 𝐷(𝑊dev, 𝑊̅̅̅̅̅̅dev) is the damage factor which is input as the table, TBHYS. This table consists of curves giving stress reduction (between 0 and 1) as a func- tion of 𝑊dev indexed by 𝑊̅̅̅̅̅̅dev. Each 𝑊̅̅̅̅̅̅dev curve must be valid for strain energy densities between 0 and 𝑊̅̅̅̅̅̅dev. It is recommended that each curve be monotonically increasing, and it is required that each curve equals 1 when 𝑊dev > 𝑊̅̅̅̅̅̅dev. Additionally, *DEFINE_TABLE requires that each curve have the same beginning and end point and, further- more, that they not cross except at the boundaries, although they are not re- quired to cross. This table can be estimated from a uniaxial quasistatic compression test as fol- lows: a) Load the specimen to a maximum displacement 𝑑 ̅ and measure the force as function of displacement: 𝑓load(𝑑 ̅). b) Unload the specimen again measuring the force as a function of displace- ment: 𝑓unload(𝑑). c) The strain energy density is, then, given as a function of the loaded dis- placement as 𝑊dev(𝑑) = ∫ 𝑓load(𝑠)𝑑𝑠 . i) ii) The peak energy, which is used to index the data set, is given by 𝑊̅̅̅̅̅̅dev = 𝑊dev(𝑑 ̅). From this energy curve we can also determine the inverse: 𝑑(𝑊dev). Using this inverse the load curve for LS-DYNA is then given by: 𝐷(𝑊dev, 𝑊̅̅̅̅̅̅dev) = 𝑓unload[𝑑(𝑊dev)] 𝑓load[𝑑(𝑊dev)] . d) This procedure is repeated for different values of 𝑑 ̅ (or equivalently 𝑊̅̅̅̅̅̅dev). 2. Hysteresis (TBHYS < 0). If a negative table ID for hysteresis is defined, then all of the above holds. The difference being that the load curves comprising table, |TBHYS|, must give the strain-energy density, 𝑊dev, as a function of the stress reduction factor. This scheme guarantees that all curves have the same begin- ning point, 0, and the same end point, 1. For negative TBHYS the user provides 𝑊dev(𝐷, 𝑊̅̅̅̅̅̅dev) instead of 𝐷(𝑊dev, 𝑊̅̅̅̅̅̅dev). In practice, this case corresponds to swapping the load curve axes. *MAT_OGDEN_RUBBER This is also Material Type 77. This material model provides the Ogden [1984] rubber model combined optionally with linear viscoelasticity as outlined by Christensen [1980]. Card 1 1 Variable MID 2 RO Type A8 F 3 PR F 4 N I 5 NV I 6 G F 7 8 SIGF REF F F Hysteresis Card. Additional card read in when PR < 0 (Mullins Effect). Card 2 1 2 3 4 5 6 7 8 Variable TBHYS Type F Card 3 for N > 0. For N > 0 a least squares fit is computed from uniaxial data. Card 3 1 Variable SGL 2 SW Type F F 3 ST F 4 5 6 7 8 LCID1 DATA LCID2 BSTART TRAMP F F F F Card 3 for N = 0. Set the material parameters directly. Card 3 1 2 3 4 5 6 7 8 Variable MU1 MU2 MU3 MU4 MU5 MU6 MU7 MU8 Type F F F F F F F Card 4 for N = 0. Set the material parameters directly. Card 4 1 2 3 4 5 6 7 8 Variable ALPHA1 ALPHA2 ALPHA3 ALPHA4 ALPHA5 ALPHA6 ALPHA7 ALPHA8 Type F F F F F F F F Optional Viscoelastic Constants Cards. Up to 12 cards may be input. A keyword card (with a “*” in column 1) terminates this input if less than 12 cards are used. 1 GI F Card 5 Variable Type Default 2 3 4 5 6 7 8 BETAI VFLAG F I 0 VARIABLE DESCRIPTION MID RO PR N Material identification. A unique number or label not exceeding 8 characters must be specified. Mass density Poisson’s ratio (≥ 49 is recommended; smaller values may not work and should not be used). If this is set to a negative number, then the absolute value is used and an extra card is read for Mullins effect. Order of fit to the Ogden model, (currently < 9, 2 generally works okay). The constants generated during the fit are printed in the output file and can be directly input in future runs, thereby, saving the cost of performing the nonlinear fit. The users need to check the correction of the fit results before proceeding to compute. VARIABLE NV G SIGF REF DESCRIPTION Number of Prony series terms in fit. If zero, the default is 6. Currently, the maximum number is set to 12. Values less than 12, possibly 3-5 are recommended, since each term used adds significantly to the cost. Caution should be exercised when taking the results from the fit. Preferably, all generated coefficients should be positive. Negative values may lead to unstable results. Once a satisfactory fit has been achieved it is recommended that the coefficients which are written into the output file be input in future runs. Shear modulus for frequency independent damping. Frequency independent damping is based on a spring and slider in series. The critical stress for the slider mechanism is SIGF defined below. For the best results, the value of G should be 250-1000 times greater than SIGF. Limit stress for frequency independent frictional damping. Use reference geometry to initialize the stress tensor. The reference geometry is defined by the keyword: *INITIAL_- FOAM_REFERENCE_GEOMETRY . EQ.0.0: off, EQ.1.0: on. TBHYS Table ID for hysteresis, could be positive or negative, see Remarks on *MAT_HYPERELASTIC_RUBBER If N > 0 test information from a uniaxial test are used: SGL SW ST LCID1 Specimen gauge length Specimen width Specimen thickness Load curve ID giving the force versus actual change in the gauge length. If SGL, SW, and ST are set to unity (1.0), then curve LCID1 is also engineering stress versus engineering strain. VARIABLE DESCRIPTION DATA Type of experimental data. EQ.1.0: uniaxial data (default) EQ.2.0: biaxial data EQ.3.0: pure shear data LCID2 Load curve ID of the deviatoric stress relaxation curve, neglecting the long term deviatoric stress. If LCID2 is given, constants 𝐺𝑖 and 𝛽𝑖 are determined via a least squares fit. See M76-1 for an example relaxation curve. The ordinate of the curve is the viscoelastic deviatoric stress divided by (2 times the constant value of deviatoric strain) where the stress and strain are in the direction of the prescribed strain, or in non-directional terms, the effective stress divided by (3 times the effective strain). BSTART In the fit, 𝛽𝑖 is set to zero, 𝛽2 is set to BSTART, 𝛽3 is 10 times 𝛽2, 𝛽4 is 10 times 𝛽3 , and so on. If zero, BSTART is determined by an iterative trial and error scheme. TRAMP Optional ramp time for loading. MUi 𝜇𝑖, the ith shear modulus, i varies up to 8. See discussion below. ALPHAi 𝛼𝑖, the ith exponent, i varies up to 8. See discussion below. Gi Optional shear relaxation modulus for the ith term BETAi Optional decay constant if ith term Flag for the viscoelasticity formulation. This appears only on the first line defining Gi, BETAi, and VFLAG. If VFLAG = 0, the standard viscoelasticity formulation is used (the default), and if the viscoelasticity the VFLAG = 1, instantaneous elastic stress is used. formulation using VFLAG Remarks: Rubber is generally considered to be fully incompressible since the bulk modulus greatly exceeds the shear modulus in magnitude. To model the rubber as an unconstrained material a hydrostatic work term is included in the strain energy functional which is function of the relative volume, 𝐽, [Ogden 1984]: 𝑊∗ = ∑ ∑ 𝑗=1 𝑖=1 𝜇𝑗 𝛼𝑗 ∗𝛼𝑗 − 1) + 𝐾(𝐽 − 1 − ln𝐽) (𝜆𝑖 The asterisk (*) indicates that the volumetric effects have been eliminated from the ∗. The number of terms, n, may vary from 1 to 8 inclusive, and 𝐾 is principal stretches, 𝜆𝑗 the bulk modulus. Rate effects are taken into account through linear viscoelasticity by a convolution integral of the form: 𝜎𝑖𝑗 = ∫ 𝑔𝑖𝑗𝑘𝑙(𝑡 − 𝜏) ∂𝜀𝑘𝑙 ∂𝜏 𝑑𝜏 or in terms of the second Piola-Kirchhoff stress, 𝑆ij , and Green's strain tensor, 𝐸𝑖𝑗, 𝑆𝑖𝑗 = ∫ 𝐺𝑖𝑗𝑘𝑙(𝑡 − 𝜏) ∂𝐸𝑘𝑙 ∂𝜏 𝑑𝜏 where 𝑔𝑖𝑗𝑘𝑙(𝑡 − 𝜏) and 𝐺𝑖𝑗𝑘𝑙(𝑡 − 𝜏) are the relaxation functions for the different stress measures. This stress is added to the stress tensor determined from the strain energy functional. If we wish to include only simple rate effects, the relaxation function is represented by six terms from the Prony series: given by, 𝑔(𝑡) = 𝛼0 + ∑ 𝛼𝑚𝑒−𝛽𝑡 𝑚=1 𝑔(𝑡) = ∑ 𝐺𝑖𝑒−𝛽𝑖𝑡 𝑖=1 This model is effectively a Maxwell fluid which consists of a dampers and springs in series. We characterize this in the input by shear moduli, 𝐺𝑖, and decay constants, 𝛽𝑖. The viscoelastic behavior is optional and an arbitrary number of terms may be used. In order to avoid a constant shear modulus from this viscoelastic formulation, a term in the series is included only when 𝛽𝑖 > 0. For VFLAG = 1, the viscoelastic term is 𝜎𝑖𝑗 = ∫ 𝑔𝑖𝑗𝑘𝑙(𝑡 − 𝜏) ∂𝜎𝑘𝑙 ∂𝜏 𝑑𝜏 𝐸 is the instantaneous stress evaluated from the internal energy functional. The where 𝜎𝑘𝑙 coefficients in the Prony series therefore correspond to normalized relaxation moduli instead of elastic moduli. The Mooney-Rivlin rubber model (model 27) is obtained by specifying 𝑛 = 1. In spite of the differences in formulations with Model 27, we find that the results obtained with this model are nearly identical with those of Material 27 as long as large values of Poisson’s ratio are used. The frequency independent damping is obtained by the having a spring and slider in series as shown in the following sketch: friction *MAT_SOIL_CONCRETE This is Material Type 78. This model permits concrete and soil to be efficiently modeled. See the explanations below. Card 1 1 Variable MID Type A8 Card 2 Variable 1 PC 2 RO F 2 OUT Type F F 3 G F 3 B F 4 K F 4 FAIL F 5 6 7 8 LCPV LCYP LCFP LCRP F 5 F 6 F 7 F 8 VARIABLE DESCRIPTION MID RO G K LCPV Material identification. A unique number or label not exceeding 8 characters must be specified. Mass density Shear modulus Bulk modulus Load curve ID for pressure versus volumetric strain. The pressure versus volumetric strain curve is defined in compression only. The sign convention requires that both pressure and compressive strain be defined as positive values where the compressive strain is taken as the negative value of the natural logarithm of the relative volume. LCYP Load curve ID for yield versus pressure: GT.0: von Mises stress versus pressure, LT.0: Second stress invariant, J2, versus pressure. This curve must be defined. 1.0 Figure M78-1. Strength reduction factor. VARIABLE DESCRIPTION LCFP LCRP PC OUT Load curve ID for plastic strain at which fracture begins versus pressure. This load curve ID must be defined if B > 0.0. Load curve ID for plastic strain at which residual strength is reached versus pressure. This load curve ID must be defined if B > 0.0. Pressure cutoff for tensile fracture Output option for plastic strain in database: EQ.0: volumetric plastic strain, EQ.1: deviatoric plastic strain. B Residual strength factor after cracking, see Figure M78-1. FAIL Flag for failure: EQ.0: no failure, EQ.1: When pressure reaches failure pressure element is eroded, EQ.2: When pressure reaches failure pressure element loses it ability to carry tension. Remarks: Pressure is positive in compression. Volumetric strain is defined as the natural log of the relative volume and is positive in compression where the relative volume, V, is the *MAT_SOIL_CONCRETE Figure M78-2. Cracking strain versus pressure. ratio of the current volume to the initial volume. The tabulated data should be given in order of increasing compression. If the pressure drops below the cutoff value specified, it is reset to that value and the deviatoric stress state is eliminated. If the load curve ID (LCYP) is provided as a positive number, the deviatoric, perfectly plastic, pressure dependent, yield function φ, is given as 𝜙 = √3J2 − 𝐹(𝑝) = 𝜎𝑦 − 𝐹(𝑝) where , F(p) is a tabulated function of yield stress versus pressure, and the second invariant, J2, is defined in terms of the deviatoric stress tensor as: 𝐽2 = 𝑆𝑖𝑗𝑆𝑖𝑗 assuming that if the ID is given as negative then the yield function becomes: being the deviatoric stress tensor. 𝜙 = 𝐽2 − 𝐹(𝑝) If cracking is invoked by setting the residual strength factor, B, on card 2 to a value between 0.0 and 1.0, the yield stress is multiplied by a factor f which reduces with plastic strain according to a trilinear law as shown in Figure M78-1. 𝑏 = residual strength factor 1 = plastic stain at which cracking begins. 2 = plastic stain at which residual strength is reached. ε1 and ε2 are tabulated functions of pressure that are defined by load curves, see Figure M78-2. The values on the curves are pressure versus strain and should be entered in order of increasing pressure. The strain values should always increase monotonically with pressure. By properly defining the load curves, it is possible to obtain the desired strength and ductility over a range of pressures, see Figure M78-3. Yield stress p3 p2 p1 Figure M78-3. Yield stress as a function of plastic strain. Plastic strain *MAT_HYSTERETIC_SOIL This is Material Type 79. This model is a nested surface model with up to ten superposed “layers” of elasto-perfectly plastic material, each with its own elastic moduli and yield values. Nested surface models give hysteric behavior, as the different “layers” yield at different stresses. See Remarks below. Card 1 1 Variable MID 2 RO Type A8 F Card 2 Variable 1 DF Type F Card 3 1 2 RP F 2 3 K0 F 3 4 P0 F 4 5 B F 5 6 A0 F 6 7 A1 F 7 8 A2 F 8 LCID SFLC DIL_A DIL_B DIL_C DIL_D F 3 F 4 F 5 F 6 F 7 F 8 Variable GAM1 GAM2 GAM3 GAM4 GAM5 LCD LCSR PINIT Type F Card 4 1 F 2 F 3 F 4 F 5 I 6 I 7 I 8 Variable TAU1 TAU2 TAU3 TAU4 TAU5 Type F F F F F VARIABLE MID DESCRIPTION Material identification. A unique number or label not exceeding 8 characters must be specified. RO Mass density VARIABLE DESCRIPTION K0 P0 B A0 A1 A2 DF RP LCID Bulk modulus at the reference pressure Cut-off/datum pressure (must be 0≤ i.e. tensile). Below this pressure, stiffness and strength disappears; this is also the “zero” pressure for pressure-varying properties. B is the exponent for the pressure-sensitive elastic moduli. See remarks. B must be in the range 0 ≤ 𝐵 < 1, and values too close to 1 are not recommended because the pressure becomes indeterminate. Yield function constant a0 (Default = 1.0), see Material Type 5. Yield function constant a1 (Default = 0.0), see Material Type 5. Yield function constant a2 (Default = 0.0), see Material Type 5. Damping factor. Must be in the range 0≤df≤1: EQ.0: no damping, EQ.1: maximum damping. Reference pressure for following input data. Load curve ID defining shear strain verses shear stress. Up to ten points may be defined in the load curve. See *DEFINE_CURVE. SFLD Scale factor to apply to shear stress in LCID. DIL_A DIL_B DIL_C DIL_D GAM1 GAM2 GAM3 GAM4 Dilation parameter A Dilation parameter B Dilation parameter C Dilation parameter D γ1, shear strain (ignored if LCID is non zero). γ2, shear strain (ignored if LCID is non zero). γ3, shear strain (ignored if LCID is non zero). γ4, shear strain (ignored if LCID is non zero). GAM5 LCD LCSR *MAT_HYSTERETIC_SOIL DESCRIPTION γ5, shear strain (ignored if LCID is non zero). strain amplitudes Optional Load Curve ID defining damping ratio of hysteresis at different for unload/reload). The x-axis is shear strain, the y-axis is the damping ratio (e.g., 0.05 for 5% damping). The strains (x-axis values) of curve LCD must be identical to those of curve LCID. (overrides Masing rules Load curve ID defining plastic strain rate scaling effect on yield stress. See *DEFINE_CURVE. The x-axis is plastic strain rate, the y-axis is the yield enhancement factor. PINIT Flag for pressure sensitivity (B and A0, A1, A2 equations): EQ.0: Use current pressure (will vary during the analysis) EQ.1: Use pressure from initial stress state EQ.2: Use initial “plane stress” pressure (𝜎𝑣 + 𝜎ℎ)/2 EQ.3: User (compressive) initial vertical stress τ1, shear stress at γ1 (ignored if LCID is non zero). τ2, shear stress at γ2 (ignored if LCID is non zero). τ3, shear stress at γ3 (ignored if LCID is non zero). τ4, shear stress at γ4 (ignored if LCID is non zero). τ5, shear stress at γ5 (ignored if LCID is non zero). TAU1 TAU2 TAU3 TAU4 TAU5 Remarks: The elastic moduli G and K are pressure sensitive: 𝐺(𝑝) = 𝐾(𝑝) = 𝐺0(𝑝 − 𝑝0)𝑏 (𝑝ref − 𝑝0)𝑏 𝐾0(𝑝 − 𝑝0)𝑏 (𝑝ref − 𝑝0)𝑏 where G0 and K0 are the input values, p is the current pressure, p0 the cut-off or datum pressure (must be zero or negative). If p attempts to fall below p0 (i.e., more tensile) the shear stresses are set to zero and the pressure is set to p0. Thus, the material has no stiffness or strength in tension. The pressure in compression is calculated as follows: 𝑝 = 𝑝ref [− ⁄ (1−𝑏) 𝐾0 𝑝ref ln(𝑉)] where V is the relative volume, i.e., the ratio between the original and current volume. This formula results in an instantaneous bulk modulus proportional to pb whose value at the reference pressure is equal to K0/(1-b). The constants a0, a1, a2 govern the pressure sensitivity of the yield stress. Only the ratios between these values are important - the absolute stress values are taken from the stress-strain curve. The stress strain pairs define a shear stress versus shear strain curve. The first point on the curve is assumed by default to be (0,0) and does not need to be entered. The slope of the curve must decrease with increasing γ. This curves applies at the reference pressure; at other pressures the curve is scaled by 𝜏(𝑝, 𝛾) 𝜏(𝑝𝑟𝑒𝑓 , 𝛾) = √ [𝑎0 + 𝑎1(𝑝 − 𝑝0) + 𝑎2(𝑝 − 𝑝0)2] [𝑎0 + 𝑎1(𝑝ref − 𝑝0) + 𝑎2(𝑝ref − 𝑝0)2] The shear stress-strain curve (with points (τ1,γ1), (τ2,γ2)...(τN,γN)) is converted into a series of N elastic perfectly-plastic curves such that ∑(𝜏𝑖, (𝛾)) = 𝜏(𝛾), as shown in the figure below. elasto-plastic 1 elasto-plastic 2 shear strain elasto-plastic 3 elasto-plastic 4 Figure M79-1. low pressure Each elastic perfectly-plastic curve represents one “layer” in the material model. Deviatoric stresses are stored and calculated separately for each layer. The total deviatoric stress is the sum of the deviatoric stresses in each layer. By this method, hysteretic (energy-absorbing) stress-strain curves are generated in response to any strain cycle of amplitude greater than the lowest yield strain of any layer. The example below shows response to small and large strain cycles (blue and pink lines) superposed on the input curve (thick red line). ) ( 60 40 20 -20 -40 -60 backbone curve shear strain amplitude: 0.16% shear strain amplitude: 0.06% -0.2 -0.1 0.1 0.2 0.3 0.4 shear strain % Figure M79-2. Definition of shear strain and shear stress: Different definitions of “shear strain” and “shear stress” are possible when applied to the three-dimensional stress states. MAT_079 uses the following definitions: Input shear stress is treated by the material model as, 0.5 × Von Mises Stress = √(3𝜎′𝑖: 𝜎′𝑖 8⁄ ). Input shear strain is treated by the material model as 1.5 × Von Mises Strain = √(3𝜀′𝑖: 𝜀′𝑖 2⁄ ). For a particular stress or strain state (defined by the relationship between the three principal stresses or strains), a scaling factor may be needed in order to convert between the definitions given above and the shear stress or strain that an engineer would expect. The MAT_079 definitions of shear stress and shear strain are derived from triaxial testing in which one principal stress is applied, while the other two principal stresses are equal to a confining stress which is held constant, i.e. principal stresses and strains have the form (a, b, b). If instead the user wishes the input curve to represent a test in which a pure shear strain is applied over a hydrostatic pressure, such as a shear-box text, then it is recommended to scale both the x-axis and the y-axis of the curve by 0.866. This factor assumes principal stresses of the form (p+t, p-t, p) where t is the applied shear stress, and similar for the principal strains. Pressure Sensitivity: The yield stresses of the layers, and hence the stress at each point on the shear stress- strain input curve, vary with pressure according to constants A0, A1 and A2. The elastic moduli, and hence also the slope of each section of shear stress-strain curve, vary with pressure according to constant B. These effects combine to modify the shear stress-strain curve according to pressure: 1 ≠ θ 2, slope varies with pressure according to B stress varies with pressure according to A0, A1, and A2 at different P, same point on the input stress-strain curve will be reached at different strain high pressure (P2) low pressure (P1) shear strain Figure M79-3. Pressure sensitivity can make the solution sensitive to numerical noise. In cases where the expected pressure changes are small compared to the initial stress state, it may be preferable to use pressure from the initial stress state instead of current pressure as the basis for the pressure sensitivity (option PINIT). This causes the bulk modulus and shear stress-strain curve to be calculated once for each element at the start of the analysis and to remain fixed thereafter. PINIT affects both stiffness (calculated using B) and strength (calculated using A0, A1 and A2). If PINIT options 2 (“plane stress” pressure) or 3 (vertical stress) are used, these quantities substitute for pressure p in the equations above. Input values of pref and p0 should then also be “plane stress” pressure or vertical stress, respectively. If PINIT is used, B is allowed to be as high as 1.0 (stiffness proportional to initial pressure); otherwise, values of B higher than about 0.5 are not recommended. Dilatancy: Parameters DIL_A, DIL_B, DIL_C and DIL_D control the compaction and dilatancy that occur in sandy soils as a result of shearing motion. The dilatancy is expressed as a volume strain γv: 𝜀v = 𝜀r + 𝜀g 𝜀r = DIL_ A(Γ)DIL_ B 𝜀g = ∫(𝑑𝛾𝑥𝑧 2⁄ 2 ) 2 + 𝑑𝛾𝑦𝑧 DIL_ C + DIL_ D × ∫(𝑑𝛾𝑥𝑧 2⁄ 2 ) 2 + 𝑑𝛾𝑦𝑧 Γ = (𝛾𝑥𝑧 2⁄ 2 ) 2 + 𝛾𝑦𝑧 𝛾𝑥𝑧 = 2𝜀𝑥𝑧 𝛾𝑦𝑧 = 2𝜀𝑦𝑧 γr describes the dilation of the soil due to the magnitude of the shear strains; this is caused by the soil particles having to climb over each other to develop shear strain. γg describes compaction of the soil due to collapse of weak areas and voids, caused by continuous shear straining. Recommended inputs for sandy soil: DIL_A DIL_B DIL_C DIL_D - 10 - 1.6 - 100 - 2.5 DIL_A and DIL_B may cause instabilities in some models. If this facility is used with pore water pressure, liquefaction can be modeled. Strain rate sensitivity: Strain rate effect is accounted for by scaling the yield stress of each layer as the user- specified function of plastic strain rate. The stress-strain curve defined by LCID is considered as the reference curve or the curve for the lowest shear strength among all plastic strain rates. Scale factor versus strain rate is defined in curve LCSR. All scale factors must be equal to or larger than 1.0. For a given plastic strain rate, the effective scale factor for the resultant stress (instead of layer stresses) is 1.0 for elastic range and ramping up to the one corresponding to the given plastic strain rate when the stress is approaching the ultimate yield stress (last point of curve LCID). *MAT_RAMBERG-OSGOOD This is Material Type 80. This model is intended as a simple model of shear behavior and can be used in seismic analysis. Card 1 1 Variable MID 2 RO 3 4 5 GAMY TAUY ALPHA Type A8 F F F F 6 R F 7 8 BULK F Default none none none none none none none VARIABLE MID DESCRIPTION Material identification. A unique number or label not exceeding 8 characters must be specified. RO Mass density. GAMY TAUY Reference shear strain (γy) Reference shear stress (τy) ALPHA Stress coefficient (α) R Stress exponent (r) BULK Elastic bulk modulus Remarks: The Ramberg-Osgood equation is an empirical constitutive relation to represent the one-dimensional elastic-plastic behavior of many materials, including soils. This model allows a simple rate independent representation of the hysteretic energy dissipation observed in soils subjected to cyclic shear deformation. For monotonic loading, the stress-strain relationship is given by: 𝛾𝑦 𝛾𝑦 = = 𝜏𝑦 𝜏𝑦 ∣ ∣ + 𝛼 ∣ 𝜏𝑦 − 𝛼 ∣ 𝜏𝑦 , for 𝛾 ≥ 0 , for 𝛾 < 0 where 𝛾 is the shear and 𝜏 is the stress. The model approaches perfect plasticity as the stress exponent 𝑟 → ∞. These equations must be augmented to correctly model unloading and reloading material behavior. The first load reversal is detected by 𝛾𝛾̇ < 0. After the first reversal, the stress-strain relationship is modified to (𝛾 − 𝛾0) 2𝛾𝑦 (𝛾 − 𝛾0) 2𝛾𝑦 = = (𝜏 − 𝜏0) 2𝜏𝑦 (𝜏 − 𝜏0) 2𝜏𝑦 + 𝛼 ∣ − 𝛼 ∣ ′ (𝜏 − 𝜏0) ∣ 2𝜏𝑦 ′ (𝜏 − 𝜏0) ∣ 2𝜏𝑦 , for 𝛾 ≥ 0 , for 𝛾 < 0 where 𝛾0 and 𝜏0 represent the values of strain and stress at the point of load reversal. Subsequent load reversals are detected by (𝛾 − 𝛾0)𝛾̇ < 0. The Ramberg-Osgood equations are inherently one-dimensional and are assumed to apply to shear components. To generalize this theory to the multidimensional case, it is assumed that each component of the deviatoric stress and deviatoric tensorial strain is independently related by the one-dimensional stress-strain equations. A projection is used to map the result back into deviatoric stress space if required. The volumetric behavior is elastic, and, therefore, the pressure p is found by where 𝜀𝑣 is the volumetric strain. 𝑝 = −𝐾𝜀𝑣 *MAT_PLASTICITY_WITH_DAMAGE_{OPTION} This manual entry apply to both types 81 and 82. Materials 81 and 82 model an elasto- visco-plastic material with user-defined isotropic stress versus strain curves, which, themselves, may be strain-rate dependent. This model accounts for the effects of damage prior to rupture based on an effective plastic-strain measure. Additionally, failure can be triggered when the time step drops below some specified value. Available options include: <BLANK> ORTHO ORTHO_RCDC ORTHO_RCDC1980 STOCHAS The ORTHO option invokes an orthotropic damage model, an extension that was first added as for modelling failure in aluminum panels. Directional damage begins after a defined failure strain is reached in tension and continues to evolve until a tensile rupture strain is reached in either one of the two orthogonal directions. After rupture is detected at all integration points, the element is deleted. The ORTHO_RCDC option invokes the damage model developed by Wilkins [Wilkins, et al. 1977]. The ORTHO_RCDC1980 option invokes a damage model based on strain invariants as developed by Wilkins [Wilkins, et al. 1980]. A nonlocal formulation, which requires additional storage, is used if a characteristic length is defined. The RCDC option, which was added at the request of Toyota, works well in predicting failure in cast aluminum; see Yamasaki, et al., [2006]. NOTE: This keyword, in its long form, *MAT_PLASTICI- TY_WITH_DAMAGE, with no options invokes ma- terial type 81. Adding an orthotropic damage option will invoke material type 82. Since type 82 must track directional strains it is, computationally, more expensive. Card 1 1 Variable MID 2 RO Type A8 F 3 E F 4 PR F 5 6 7 8 SIGY ETAN EPPF TDEL F F F F Default none none none none none 0.0 1012 0.0 Card 2 Variable Type Default 1 C F 0 Card 3 1 2 P F 0 2 3 4 5 LCSS LCSR EPPFR F 0 3 F 0 4 F 1014 5 6 VP F 0 6 7 8 LCDM NUMINT F 0 7 I 0 8 Variable EPS1 EPS2 EPS3 EPS4 EPS5 EPS6 EPS7 EPS8 Type Default F 0 Card 4 1 F 0 2 F 0 3 F 0 4 F 0 5 F 0 6 F 0 7 F 0 8 Variable ES1 ES2 ES3 ES4 ES5 ES6 ES7 ES8 Type Default F 0 F 0 F 0 F 0 F 0 F 0 F 0 F Ortho RCDC Card. Additional card for keyword option ORTHO_RCDC. Card 5 1 2 3 4 Variable ALPHA BETA GAMMA D0 Type Default F 0 F 0 F 0 F 0 5 B F 0 6 7 LAMBDA DS F 0 F 0 8 L F 0 VARIABLE DESCRIPTION MID RO E PR SIGY ETAN EPPF TDEL C P Material identification. A unique number or label not exceeding 8 characters must be specified. Mass density. Young’s modulus. Poisson’s ratio. Yield stress. Tangent modulus, ignored if (LCSS.GT.0) is defined. 𝜀failure , effective plastic strain at which material softening begins. Minimum time step size for automatic element deletion. Strain rate parameter, 𝐶, see formula below. Strain rate parameter, 𝑃, see formula below. LCSS Load curve ID or Table ID. 1. Case 1: LCSS is a load curve ID. The load curve LCSS maps effective plastic strain to effective stress. If the fields EPS1 - EPS8 and ES1 - ES8 are defined, they are ignored. 2. Case 2: LCSS is a Table ID. Each strain rate value is associated to a load curve ID giving the stress as a func- tion of effective plastic strain for that rate, See Figure M24-1. The stress versus effective plastic strain curve for the lowest value of strain rate is used if the strain rate falls below the minimum value. Likewise, the stress VARIABLE DESCRIPTION versus effective plastic strain curve for the highest value of strain rate is used if the strain rate exceeds the maxi- mum value. The strain rate parameters: C and P; the curve ID, LCSR; EPS1 - EPS8 and ES1 - ES8 are ignored if a Table ID is defined. The strain rate values defined in the table may be given as the natural logarithm of the strain rate. If the first stress-strain curve in the table corresponds to a negative strain rate, LS-DYNA assumes that the natural logarithm of the strain rate value is used. Since the tables are inter- nally discretized to equally space the points, natural logarithms are necessary, for example, if the curves corre- spond to rates from 10−4 to 104. LCSR Load curve ID defining strain rate scaling effect on yield stress. EPPFR 𝜀rupture , effective plastic strain at which material ruptures. VP Formulation for rate effects: EQ.0.0: Scale yield stress (default), EQ.1.0: Viscoplastic formulation. LCDM NUMINT Optional curve ID defining nonlinear damage curve. To activate the damage curve either the EPPF or EPPFR fields must contain nonzero values. Number of through thickness integration points which must fail before a shell element is deleted. (If zero, all points must fail.) The default of all integration points is not recommended since shells undergoing large strain are often not deleted due to nodal fiber rotations which limit strains at active integration points after most points have failed. Better results are obtained if NUMINT is set to 1 or a number less than one half of the number of through thickness points. For example, if four through thickness points are used, NUMINT should not exceed 2, even for fully integrated shells which have 16 integration points. EPS1 - EPS8 Effective plastic strain values (optional if SIGY is defined). At least 2 points should be defined. ES1 - ES8 Corresponding yield stress values to EPS1 - EPS8. yield stress versus effective plastic strain for undamaged material failure begins nominal stress after failure damage, ω, increases linearly with plastic strain after failure rupture Figure M81-1. Stress strain behavior when damage is included VARIABLE DESCRIPTION ALPHA Parameter 𝛼. for the Rc-Dc model BETA Parameter 𝛽. for the Rc-Dc model GAMMA Parameter 𝛾. for the Rc-Dc model D0 B Parameter 𝐷0. for the Rc-Dc model Parameter 𝑏. for the Rc-Dc model LAMBDA Parameter 𝜆. for the Rc-Dc model Parameter 𝐷𝑠. for the Rc-Dc model Optional characteristic element length for this material. We recommend that the default of 0 always be used, especially in parallel runs. If zero, nodal values of the damage function are used to compute the damage gradient. See discussion below. DS L Remarks: The stress strain behavior may be treated by a bilinear stress strain curve by defining the tangent modulus, ETAN. Alternately, a curve similar to that shown in Figure M24-1 is expected to be defined by (EPS1, ES1) - (EPS8, ES8); however, an effective stress versus effective plastic strain curve (LCSS) may be input instead if eight points are insufficient. The cost is roughly the same for either approach. The most general approach is to use the table definition (LCSS) discussed below. Three options to account for strain rate effects are possible: 1. Strain rate may be accounted for using the Cowper and Symonds model which scales the yield stress with the factor 1 + ( 6⁄ ) 𝜀̇ where 𝜀̇ is the strain rate, 𝜀̇ = √𝜀̇𝑖𝑗𝜀̇𝑖𝑗. If the viscoplastic option is active, VP = 1.0, and if SIGY is > 0 then the dynamic 𝑝 ), which is yield stress is computed from the sum of the static stress, 𝜎𝑦 typically given by a load curve ID, and the initial yield stress, SIGY, multiplied by the Cowper-Symonds rate term as follows: 𝑠(𝜀eff 𝜎𝑦(𝜀eff 𝑝 , 𝜀̇eff 𝑝 ) = 𝜎𝑦 𝑠(𝜀eff 𝑝 ) + SIGY × 𝑝⁄ 𝜀̇eff ⎟⎞ 𝐶 ⎠ ⎜⎛ ⎝ where the plastic strain rate is used. With this latter approach similar results can be obtained between this model and material model: *MAT_ANISOTROP- IC_VISCOPLASTIC. If SIGY = 0, the following equation is used instead where 𝑝 ), must be defined by a load curve: the static stress, 𝜎𝑦 𝑠(𝜀eff 𝜎𝑦(𝜀eff 𝑝 , 𝜀̇eff 𝑝 ) = 𝜎𝑦 𝑝 ) 𝑠(𝜀eff 𝜀̇eff ⎟⎞ 𝐶 ⎠ ⎜⎛ ⎝ ⎡ 1 + ⎢⎢ ⎣ 𝑝⁄ ⎤ ⎥⎥ ⎦ This latter equation is always used if the viscoplastic option is off. 2. For complete generality a load curve (LCSR) to scale the yield stress may be input instead. In this curve the scale factor versus strain rate is defined. 3. If different stress versus strain curves can be provided for various strain rates, the option using the reference to a table (LCSS) can be used. Then the table input in *DEFINE_TABLE is expected, see Figure M24-1. The constitutive properties for the damaged material are obtained from the undamaged material properties. The amount of damage evolved is represented by the constant, 𝜔, which varies from zero if no damage has occurred to unity for complete rupture. For uniaxial loading, the nominal stress in the damaged material is given by 𝜎nominal = failure Figure M81-2. A nonlinear damage curve is optional. Note that the origin of the curve is at (0,0). It is permissible to input the failure strain EPPF as zero for this option. The nonlinear damage curve is useful for controlling the softening behavior after the failure strain is reached. where P is the applied load and A is the surface area. The true stress is given by: where 𝐴loss is the void area. The damage variable can then be defined: 𝜎true = 𝐴 − 𝐴loss such that 𝜔 = 𝐴loss 0 ≤ 𝜔 ≤ 1. In this model, unless LCDM is defined by the user, damage is defined in terms of effective plastic strain after the failure strain is exceeded as follows: 𝑝 − 𝜀failure 𝜀eff − 𝜀failure 𝜀rupture 𝑝 ≤ 𝜀rupture 𝜀failure ≤ 𝜀eff 𝜔 = , After exceeding the failure strain softening begins and continues until the rupture strain is reached. The Rc-Dc model is defined as: The damage D is given by where 𝜀𝑝 is the effective plastic strain, 𝐷 = ∫ 𝜔1𝜔2𝑑𝜀𝑝 𝜔1 = ( 1 − 𝛾𝜎m ) is a triaxial stress weighting term and 𝜔2 = (2 − 𝐴𝐷)𝛽 is a asymmetric strain weighting term. In the above 𝜎m is the mean stress. For 𝐴𝐷 we use 𝐴𝐷 = min (∣ 𝜎2 𝜎3 ∣ , ∣ 𝜎3 𝜎2 ∣) where 𝜎𝑖 are the principal stresses and 𝜎1 > 𝜎2 > 𝜎3. Fracture is initiated when the accumulation of damage is where 𝐷𝑐 is the a critical damage given by 𝐷𝑐 > 1 A fracture fraction, 𝐷𝑐 = 𝐷0(1 + 𝑏|∇𝐷|𝜆) 𝐹 = 𝐷 − 𝐷𝑐 𝐷𝑠 defines the degradations of the material by the Rc-Dc model. For the Rc-Dc model the gradient of damage needs to be estimated. The damage is connected to the integration points, and, thus, the computation of the gradient requires some manipulation of the LS-DYNA source code. Provided that the damage is connected to nodes, it can be seen as a standard bilinear field and the gradient is easily obtained. To enable this, the damage at the integration points are transferred to the nodes as follows. Let 𝐸𝑛 be the set of elements sharing node 𝑛, 𝐸𝑛 the number of elements in that set, 𝑃𝑒 the set of integration points in element 𝑒 and ∣𝑃𝑒∣ the number of points in that set. The average damage 𝐷̅̅̅̅̅ 𝑒 in element 𝑒 is computed as 𝐷̅̅̅̅̅ 𝑒 = ∑ 𝐷𝑝 𝑝∈𝑃𝑒 ∣𝑃𝑒∣ where 𝐷𝑝 is the damage in integration point 𝑝. Finally, the damage value in node 𝑛 is estimated as 𝐷𝑛 = ∑ 𝐷̅̅̅̅̅ 𝑒 𝑒∈𝐸𝑛 |𝐸𝑛| . This computation is performed in each time step and requires additional storage. Currently we use three times the total number of nodes in the model for this calculation, but this could be reduced by a considerable factor if necessary. There is an Rc-Dc option for the Gurson dilatational-plastic model. In the implementation of this model, 𝑙 be the set of elements from the norm of the gradient is computed differently. Let 𝐸𝑓 𝑙 ∣ be the within a distance 𝑙 of element, 𝑓 not including the element itself, and let ∣𝐸𝑓 number of elements in that set. The norm of the gradient of damage is estimated roughly as ‖∇𝐷‖𝑓 ≈ 𝑙 ∣ ∣𝐸𝑓 ∑ 𝑒∈𝐸𝑓 ∣𝐷𝑒 − 𝐷𝑓 ∣ 𝑑𝑒𝑓 where 𝑑𝑒𝑓 is the distance between element 𝑓 and 𝑒. The reason for taking the first approach is that it should be a better approximation of the gradient, it can for one integration point in each element be seen as a weak gradient of an elementwise constant field. The memory consumption as well as computational work should not be much higher than for the other approach. The RCDC1980 model is identical to the RCDC model except the expression for 𝐴𝐷is in terms of the principal stress deviators and takes the form 𝐴𝐷 = max (∣ 𝑆2 𝑆3 ∣ , ∣ 𝑆2 𝑆1 ∣) The STOCHASTIC option allows spatially varying yield and failure behavior. See *DE- FINE_STOCHASTIC_VARIATION for additional information. *DEFINE_MATERIAL_HISTORIES Properties Label Attributes Description Instability Plastic Strain Rate Damage - - - - - - - - - - - 𝑝 , see EPPF Failure indicator 𝜀eff 𝑝 Effective plastic strain rate 𝜀̇eff 𝑝 /𝜀fail - Damage 𝜔 *MAT_FU_CHANG_FOAM_{OPTION} This is Material Type 83. Available options include: DAMAGE_DECAY LOG_LOG_INTERPOLATION Rate effects can be modeled in low and medium density foams, see Figure M83-1. Hysteretic unloading behavior in this model is a function of the rate sensitivity with the most rate sensitive foams providing the largest hysteresis and vice versa. The unified constitutive equations for foam materials by Chang [1995] provide the basis for this model. The mathematical description given below is excerpted from the reference. Further improvements have been incorporated based on work by Hirth, Du Bois, and Weimar [1998]. Their improvements permit: load curves generated by drop tower test to be directly input, a choice of principal or volumetric strain rates, load curves to be defined in tension, and the volumetric behavior to be specified by a load curve. The unloading response was generalized by Kolling, Hirth, Erhart and Du Bois [2006] to allow the Mullin’s effect to be modeled, i.e., after the first loading and unloading, further reloading occurs on the unloading curve. If it is desired to reload on the loading curves with the new generalized unloading, the DAMAGE decay option is available which allows the reloading to quickly return to the loading curve as the damage parameter decays back to zero in tension and compression. Card 1 1 Variable MID 2 RO Type A8 F 3 E F 4 KCON F 5 TC F 6 7 8 FAIL DAMP TBID F F F Default none none none none 1.E+20 none 0.05 none Remarks > > > ε tensile Optional Tensile Behavior TFLAG = 1 compressive Nominal Strain Default Tensile Behavior TFLAG = 0 Figure M83-1. Rate effects in the nominal stress versus engineering strain curves, which are used to model rate effects in Fu Chang’s foam model. Card 2 1 2 3 4 5 6 7 Variable BVFLAG SFLAG RFLAG TFLAG PVID SRAF REF Type F F F F F F F 8 HU F Default 1.0 0.0 0.0 0.0 0.0 0.0 0.0 0.0 Remarks 1 2 3 4 Card 3 for DAMAGE_DECAY keyword option. Card 3 1 2 3 4 5 6 7 8 Variable MINR MAXR SHAPE BETAT BETAC Type F F F F F Default 0.0 0.0 0.0 0.0 0.0 Card 3 for keyword option NOT set to DAMAGE_DECAY. Card 3 Variable 1 D0 Type F 2 N0 F 3 N1 F 4 N2 F 5 N3 F 6 C0 F 7 C1 F 8 C2 F Default 0.0 0.0 0.0 0.0 0.0 0.0 0.0 0.0 Card 4 for keyword option NOT set to DAMAGE_DECAY. Card 4 Variable 1 C3 Type F 2 C4 F 3 C5 F 4 AIJ 5 SIJ 6 7 8 MINR MAXR SHAPE F F F F F Default 0.0 0.0 0.0 0.0 0.0 0.0 0.0 0.0 *MAT_FU_CHANG_FOAM Card 5 1 2 3 4 5 6 7 8 Variable EXPON RIULD Type F F Default 1.0 0.0 VARIABLE DESCRIPTION MID RO E KCON TC FAIL DAMP TBID Material identification. A unique number or label not exceeding 8 characters must be specified. Mass density Young’s modulus Optional Young's modulus used in the computation of sound speed. This will influence the time step, contact forces, hourglass stabilization forces, and the numerical damping (DAMP). EQ.0.0: KCON is set equal to the, max(𝐸, current tangent to stresss-strain curve), if TBID ≠ 0. Otherwise, if TBID = 0, KCON is set equal to the maximum slope of the stress-strain curve. Tension cut-off stress Failure option after cutoff stress is reached: EQ.0.0: tensile stress remains at cut-off value, EQ.1.0: tensile stress is reset to zero. Viscous (0.05 < recommended value < 0.50; default is 0.05). coefficient model to damping effects Table ID, see *DEFINE_TABLE, for nominal stress vs. strain data as a function of strain rate. If the table ID is provided, cards 3 and 4 may be left blank and the fit will be done internally. The Table ID can be positive or negative . If TBID < 0, enter |TBID| on the *DEFINE_TABLE keyword. VARIABLE DESCRIPTION BVFLAG Bulk viscosity activation flag, see Remark 1: EQ.0.0: no bulk viscosity (recommended), EQ.1.0: bulk viscosity active. SFLAG Strain rate flag : EQ.0.0: true constant strain rate, EQ.1.0: engineering strain rate. RFLAG Strain rate evaluation flag see Remark 3: EQ.0.0: first principal direction, EQ.1.0: principal strain rates for each principal direction, EQ.2.0: volumetric strain rate. TFLAG Tensile stress evaluation: EQ.0.0: linear in tension. EQ.1.0: input via load curves with the tensile response corresponds to negative values of stress and strain. PVID Optional load curve ID defining pressure versus volumetric strain. See Remark 4. SRAF Strain rate averaging flag. See Remark 5. LT.0.0: use exponential moving average. EQ.0.0: use weighted running average. EQ.1.0: average the last twelve values. REF HU D0 Use reference geometry to initialize the stress tensor. The reference geometry is defined by the keyword: *INITIAL_- FOAM_REFERENCE_GEOMETRY . EQ.0.0: off, EQ.1.0: on. Hysteretic unloading factor between 0 and 1 (default = 0). See also Remark 6 and Figure M83-4. material constant, see equations below. VARIABLE N0 N1 N2 N3 C0 C1 C2 C3 C4 C5 AIJ, SIJ DESCRIPTION material constant, see equations below. material constant, see equations below. material constant, see equations below. material constant, see equations below. material constant, see equations below. material constant, see equations below. material constant, see equations below. material constant, see equations below. material constant, see equations below. material constant, see equations below. material constant, see equations below. material constant, see equations below. MINR Ratemin, minimum strain rate of interest. MAXR Ratemax, maximum strain rate of interest. SHAPE BETAT BETAC EXPON Shape factor for unloading. Active for nonzero values of the hysteretic unloading factor HU. Values less than one reduces the energy dissipation and greater than one increases dissipation, see also Figure M83-2. Decay constant for damage in tension. The damage decays after loading in ceases according to 𝑒−BETAT×𝑡. Decay constant for damage in compression. The damage decays after loading in ceases according to 𝑒−BETAC×𝑡. Exponent for unloading. Active for nonzero values of the hysteretic unloading factor HU. Default is 1.0 RIULD Flag for rate independent unloading, see Remark 6. EQ.0.0: off, EQ.1.0: on. *MAT_083 The strain is divided into two parts: a linear part and a non-linear part of the strain and the strain rate becomes 𝐄(𝑡) = 𝐄𝐿(𝑡) + 𝐄𝑁(𝑡) 𝐄̇(𝑡) = 𝐄̇𝐿(𝑡) + 𝐄̇𝑁(𝑡) where 𝐄̇𝑁 is an expression for the past history of 𝐄𝑁. A postulated constitutive equation may be written as: ∞ 𝛔(𝑡) = ∫ [𝐄𝑡 𝑁(𝜏), 𝐒(𝑡)] 𝑑𝜏 where 𝐒(𝑡) is the state variable and ∫ ∞ and 𝜏=0 ∞ .𝜏=0 is a functional of all values of 𝜏 in 𝑇𝜏: 0 ≤ 𝜏 ≤ 𝑁(𝜏) = 𝐄𝑁(𝑡 − 𝜏) 𝐄𝑡 where 𝜏 is the history parameter: 𝑁(𝜏 = ∞) ⇔ the virgin material 𝐄𝑡 It is assumed that the material remembers only its immediate past, i.e., a neighborhood about 𝜏 = 0. Therefore, an expansion of 𝐄𝑡 𝑁(𝜏) in a Taylor series about 𝜏 = 0 yields: 𝑁(𝜏) = 𝐄𝑁(0) + 𝐄𝑡 ∂𝐄𝑡 ∂𝑡 (0)𝑑𝑡 Hence, the postulated constitutive equation becomes: 𝛔(𝑡) = 𝛔∗[𝐄𝑁(𝑡), 𝐄̇𝑁(𝑡), 𝐒(𝑡)] where we have replaced ∂𝐄𝑡 ∂𝑡 by 𝐄̇𝑁, and 𝛔∗ is a function of its arguments. For a special case, we may write 𝛔(𝑡) = 𝛔∗(𝐄𝑁(𝑡), 𝐒(𝑡)) 𝐄̇ 𝑁 = 𝑓 (𝐒(𝑡), 𝐬(𝑡)) which states that the nonlinear strain rate is the function of stress and a state variable which represents the history of loading. Therefore, the proposed kinetic equation for foam materials is: 𝐄̇ 𝑁 = ‖𝛔‖ 𝐷0exp {−𝑐0 [ 𝛔: 𝐒 (‖𝛔‖)2] 2𝑛0 } where 𝐷0, 𝑐0, and 𝑛0 are material constants, and 𝐒 is the overall state variable. If either 𝐷0 = 0 or 𝑐0 → ∞ then the nonlinear strain rate vanishes. 𝑆̇𝑖𝑗 = [𝑐1(𝑎𝑖𝑗𝑅 − 𝑐2𝑆𝑖𝑗)𝑃 + 𝑐3𝑊𝑛1(∥𝐄̇𝑁∥)𝑛2𝐼𝑖𝑗]𝑅 𝑛3 ∥𝐄̇𝑁∥ 𝑐5 − 1] 𝑅 = 1 + 𝑐4 [ 𝑃 = 𝛔: 𝐄̇𝑁 𝑊 = ∫ 𝛔: (𝑑𝐄) where c1, c2, c3, c4, c5, n1, n2, n3, and aij are material constants and: 2 ‖𝛔‖ = (𝜎𝑖𝑗𝜎𝑖𝑗) ∥𝐄̇∥ = (𝐸̇𝑖𝑗𝐸̇𝑖𝑗) 2 ∥𝐄̇𝑁∥ = (𝐸̇𝑁 𝑖𝑗𝐸̇𝑁 2 𝑖𝑗) In the implementation by Fu Chang the model was simplified such that the input constants 𝑎𝑖𝑗 and the state variables 𝑆𝑖𝑗 are scalars. Additional Remarks: 1. Bulk Viscosity. The bulk viscosity, which generates a rate dependent pressure, may cause an unexpected volumetric response and consequently, it is optional with this model. 2. Constant Velocity Loading. Dynamic compression tests at the strain rates of interest in vehicle crash are usually performed with a drop tower. In this test the loading velocity is nearly constant but the true strain rate, which depends on the instantaneous specimen thickness, is not. Therefore, the engineering strain rate input is optional so that the stress strain curves obtained at constant velocity loading can be used directly. See the SFLAG field. > > Current State Nominal Strain Figure M83-2. HU=0, TBID>0 3. Strain Rates with Multiaxial Loading. To further improve the response under multiaxial loading, the strain rate parameter can either be based on the princi- pal strain rates or the volumetric strain rate. See the RFLAG field. 4. Triaxial Loading. Correlation under triaxial loading is achieved by directly inputting the results of hydrostatic testing in addition to the uniaxial data. Without this additional information which is fully optional, triaxial response tends to be underestimated. See the PVID field. 5. Strain Rate Averaging. Three different options are available. The default, SRAF = 0.0, uses a weighted running average with a weight of 1/12 on the current strain rate. With the second option, SRAF = 1.0, the last twelve strain rates are averaged. The third option, SRAF < 0, uses an exponential moving average with factor |SRAF| representing the degree of weighting decrease (−1 ≤ SRAF < 0). The averaged strain rate at time 𝑡𝑛 is obtained by: averaged = |SRAF|𝜀̇𝑛 + (1 − |SRAF|)𝜀̇𝑛−1 𝜀̇𝑛 averaged 6. Unloading Response Options. Several options are available to control unloading response in MAT_083: a) HU = 0 and TBID > 0. See Figure M83-2. This is the old way. In this case the unloading response will follow the curve with the lowest strain rate and is rate-independent. The curve with lowest strain rate value (typically zero) in TBID should correspond to the unloading path of the material as measured in a quasistatic test. > > > ε Current State Nominal Strain Figure M83-3. HU = 0, TBID < 0 The quasistatic loading path then corresponds to a realistic (small) value of the strain rate. b) HU = 0 and TBID < 0 In this case the curve with lowest strain rate value (typically zero) in TBID must correspond to the unloading path of the material as meas- ured in a quasistatic test. The quasistatic loading path then corresponds to a realistic (small) value of the strain rate. At least three curves should be used in the table (one for unloading, one for quasistatic, and one or more for dynamic response). The quasistatic loading and unloading path (thus the first two curves of the table) should form a closed loop. The unloading response is given by a damage formulation for the prin- cipal stresses as follows: 𝜎𝑖 = (1 − 𝑑)𝜎𝑖 The damage parameter d is computed internally in such a way that the unloading path under uniaxial tension and compression is fitted exactly in the simulation. The unloading response is rate dependent in this case. In some cases, this rate dependence for loading and unloading can lead to noisy results. To reduce that noise, it is possible to switch to rate in- dependent unloading with RIULD = 1. > > > ε Current State Unloading curve computed internally based on HU and SHAPE Nominal Strain Figure M83-4. HU > 0, TBID > 0 c) HU > 0 and TBID > 0 No unloading curve should be provided in the table and the curve with the lowest strain rate value in TBID should correspond to the loading path of the material as measured in a quasistatic test. At least two curves should be used in the table (one for quasistatic and one or more for dy- namic response). In this case the unloading response is given by a dam- age formulation for the principal stresses as follows: 𝜎𝑖 = (1 − 𝑑)𝜎𝑖 𝑑 = (1 − 𝐻𝑈) ⎢⎡1 − ( ⎣ 𝑊cur 𝑊max SHAPE EXPON ) ⎥⎤ ⎦ where W corresponds to the current value of the hyperelastic energy per unit undeformed volume. The unloading response is rate dependent in this case. In some cases, this rate dependence for loading and unloading can lead to noisy results. To reduce that noise, it is possible to switch to rate independent unloading with RIULD = 1. The LOG_LOG_INTERPOLATION option uses log-log interpolation for table TBID in the strain rate direction. *MAT_WINFRITH_CONCRETE This is Material Type 84 with optional rate effects. The Winfrith concrete model is a smeared crack (sometimes known as pseudo crack), smeared rebar model, implemented in the 8-node single integration point continuum element, i.e., ELFORM = 1 in *SEC- TION_SOLID. It is recommended that a double precision executable be used when using this material model. Single precision may produce unstable results. This model was developed by Broadhouse and Neilson [1987], and Broadhouse [1995] over many years and has been validated against experiments. The input documenta- tion given here is taken directly form the report by Broadhouse. The Fortran subroutines and quality assurance test problems were also provided to LSTC by the Winfrith Technology Center. Rebar may be defined using the command *MAT_WINFRITH_CONCRETE_REIN- FORCEMENT which appears in the following section. Card 1 1 Variable MID 2 RO Type A8 F Card 2 Variable Type 1 E F Card 3 1 2 YS F 2 3 TM F 3 4 PR F 4 5 6 UCS UTS F 5 F 6 7 FE F 7 8 ASIZE F 8 EH UELONG RATE CONM CONL CONT F 3 F 4 F 5 F 6 F 7 F 8 Variable EPS1 EPS2 EPS3 EPS4 EPS5 EPS6 EPS7 EPS8 Type F F F F F F F Card 4 Variable 1 P1 Type F 2 P2 F 3 P3 F 4 P4 F 5 P5 F 6 P6 F 7 P7 F 8 P8 F VARIABLE DESCRIPTION MID RO TM PR UCS UTS FE Material identification. A unique number or label not exceeding 8 characters must be specified. Mass density. Initial tangent modulus of concrete. Poisson's ratio. Uniaxial compressive strength. Uniaxial tensile strength. Depends on value of RATE below. RATE.EQ.0: Fracture energy (energy per unit area dissipated in opening crack). RATE.EQ.1: Crack width at which crack-normal tensile stress goes to zero. ASIZE Aggregate size (radius). E YS EH Young's modulus of rebar. Yield stress of rebar. Hardening modulus of rebar UEONG Ultimate elongation before rebar fails. RATE Rate effects: *MAT_WINFRITH_CONCRETE DESCRIPTION EQ.0.0: Strain rate effects are included. WARNING: energy may not be conserved using this option. EQ.1.0: Strain rate effects are turned off. Crack widths are stored as extra history variables 30, 31, 32. EQ.2.0: Like RATE = 1 but includes improved crack algorithm (recommended). Crack widths are stored as extra his- tory variables 3, 4, 5. CONM GT.0: Factor to convert model mass units to kg. EQ.-1.: Mass, length, time units in model are lbf × sec2/in, inch, sec. EQ.-2.: Mass, length, time units in model are g, cm, microsec. EQ.-3.: Mass, length, time units in model are g, mm, msec. EQ.-4.: Mass, length, time units in model are metric ton, mm, sec. EQ.-5.: Mass, length, time units in model are kg, mm, msec. CONL CONM.GT.0: CONL is the conversion factor from model length units to meters. CONM.LE.0: CONL is ignored. CONT CONM.GT.0: CONL is the conversion factor from time units to seconds CONM.LE.0: CONT is ignored. EPS1, EPS2, … Volumetric strain values (natural logarithmic values), see Remarks below. A maximum of 8 values are allowed. P1, P2, … Pressures corresponding to volumetric strain values given on Card 3. Remarks: Pressure is positive in compression; volumetric strain is given by the natural log of the relative volume and is negative in compression. The tabulated data are given in order of increasing compression, with no initial zero point. If the volume compaction curve is omitted, the following scaled curve is automatically used where 𝑝1 is the pressure at uniaxial compressive failure from: 𝑝1 = 𝜎𝑐 and 𝐾 is the bulk unloading modulus computed from 𝐾 = 𝐸𝑠 3(1 − 2𝑣) where 𝐸𝑠 is the input tangent modulus for concrete and 𝑣 is Poisson's ratio. Volumetric Strain Pressure −𝑝1/𝐾 −0.002 −0.004 −0.010 −0.020 −0.030 −0.041 −0.051 −0.062 −0.094 1.00𝑝1 1.50𝑝1 3.00𝑝1 4.80𝑝1 6.00𝑝1 7.50𝑝1 9.45𝑝1 11.55𝑝1 14.25𝑝1 25.05𝑝1 Table M84-1. Default pressure versus volumetric strain curve for concrete if the curve is not defined. The Winfrith concrete model can generate an additional binary output database containing information on crack locations, directions, and widths. In order to generate the crack database, the LS-DYNA execution line is modified by adding: where crf is the desired name of the crack database, e.g., q=d3crack. q=crf LS-PrePost can display the cracks on the deformed mesh plots. To do so, read the d3plot database into LS-PrePost and then select File → Open → Crack from the top menu bar. Or, open the crack database by adding the following to the LS-PrePost execution line: where crf is the name of the crack database, e.g., q=d3crack. q=crf By default, all the cracks in visible elements are shown. You can eliminate narrow cracks from the display by setting a minimum crack width for displayed cracks. Do this by choosing Settings → Post Settings → Concrete Crack Width. From the top menu bar of LS-PrePost, choosing Misc → Model Info will reveal the number of cracked elements and the maximum crack width in a given plot state. An ASCII “aea_crack” output file is written if the command *DATABASE_BINARY_- D3CRACK command is included in the input deck. This command does not have any bearing on the aforementioned binary crack database. *MAT_WINFRITH_CONCRETE_REINFORCEMENT This is *MAT_084_REINF for rebar reinforcement supplemental to concrete defined using Material type 84. Reinforcement may be defined in specific groups of elements, but it is usually more convenient to define a two-dimensional mat in a specified layer of a specified material. Reinforcement quantity is defined as the ratio of the cross- sectional area of steel relative to the cross-sectional area of concrete in the element (or layer). These cards may follow either one of two formats below and may also be defined in any order. Option 1 (Reinforcement quantities in element groups). Card 1 1 2 3 Variable EID1 EID2 INC Type I I I 4 XR F 5 YR F 6 ZR F 7 8 Option 2 (Two dimensional layers by part ID). Option 2 is active when first entry is left blank. Card 1 1 2 3 4 5 6 7 8 Variable PID AXIS COOR RQA RQB Type blank I I F F F VARIABLE DESCRIPTION EID1 EID2 INC XR YR ZR First element ID in group. Last element ID in group Element increment for generation. 𝑥-reinforcement quantity (for bars running parallel to global 𝑥- axis). 𝑦-reinforcement quantity (for bars running parallel to global 𝑦- axis). 𝑧-reinforcement quantity (for bars running parallel to global 𝑧- axis). VARIABLE PID DESCRIPTION Part ID of reinforced elements. If PID = 0, the reinforcement is applied to all parts which use the Winfrith concrete model. AXIS Axis normal to layer. EQ.1: A and B are parallel to global 𝑦 and 𝑧, respectively. EQ.2: A and B are parallel to global 𝑥 and 𝑧, respectively. EQ.3: A and B are parallel to global 𝑥 and 𝑦, respectively. COOR Coordinate location of layer: AXIS.EQ.1: 𝑥-coordinate AXIS.EQ.2: 𝑦-coordinate AXIS.EQ.3: 𝑧-coordinate RQA RQB Reinforcement quantity (A). Reinforcement quantity (B). Remarks: 1. Reinforcement quantity is the ratio of area of reinforcement in an element to the element's total cross-sectional area in a given direction. This definition is true for both Options 1 and 2. Where the options differ is in the manner in which it is decided which elements are reinforced. In Option 1, the reinforced element IDs are spelled out. In Option 2, elements of part ID PID which are cut by a plane (layer) defined by AXIS and COOR are reinforced. *MAT_ORTHOTROPIC_VISCOELASTIC This is Material Type 86. It allows the definition of an orthotropic material with a viscoelastic part. This model applies to shell elements. NOTE: This material does not support specification of a ma- terial angle, 𝛽𝑖, for each through-thickness integra- tion point of a shell. Card 1 1 Variable MID Type A8 Card 2 Variable 1 G0 Type F Card 3 1 2 RO F 2 3 EA F 3 4 EB F 4 5 EC F 5 6 VF F 6 7 K F 7 8 8 GINF BETA PRBA PRCA PRCB F 2 F 3 F 4 F 5 Variable GAB GBC GCA AOPT MANGLE Type F Card 4 1 F 2 F 3 Variable Type F F 4 A1 F 5 A2 F 7 8 7 8 F 6 6 A3 Variable 1 V1 Type F VARIABLE MID *MAT_ORTHOTROPIC_VISCOELASTIC 2 V2 F 3 V3 F 4 D1 F 5 D2 F 6 D3 F 7 8 DESCRIPTION Material identification. A unique number or label not exceeding 8 characters must be specified. RO EA EB EC VF K G0 GINF BETA PRBA PRCA PRCB GAB GBC GCA AOPT Mass density Young’s Modulus 𝐸𝑎 Young’s Modulus 𝐸𝑏 Young’s Modulus 𝐸𝑐 Volume fraction of viscoelastic material Elastic bulk modulus 𝐺0, short-time shear modulus 𝐺∞, long-time shear modulus 𝛽, decay constant Poisson’s ratio, 𝜈𝑏𝑎 Poisson’s ratio, 𝜈𝑐𝑎 Poisson’s ratio, 𝜈𝑐𝑏 Shear modulus, 𝐺𝑎𝑏 Shear modulus, 𝐺𝑏𝑐 Shear modulus, 𝐺𝑐𝑎 Material axes option : EQ.0.0: locally orthotropic with material axes determined by element nodes 1, 2, and 4, as with *DEFINE_COORDI- VARIABLE DESCRIPTION NATE_NODES, and then rotated about the shell ele- ment normal by an angle MANGLE. EQ.2.0: globally orthotropic with material axes determined by vectors defined below, as with *DEFINE_COORDI- NATE_ECTOR. EQ.3.0: locally orthotropic material axes determined by rotating the material axes about the element normal by an angle, MANGLE, from a line in the plane of the el- ement defined by the cross product of the vector 𝐯 with the element normal. LT.0.0: the absolute value of AOPT is a coordinate system ID number (CID on *DEFINE_COORDINATE_NODES, *DEFINE_COORDINATE_SYSTEM or *DEFINE_CO- ORDINATE_VECTOR). Available in R3 version of 971 and later. MANGLE Material angle in degrees for AOPT = 0 and 3, may be overridden on the element card, see *ELEMENT_SHELL_BETA. A1 A2 A3 Define components of vector 𝐚 for AOPT = 2. V1 V2 V3 Define components of vector 𝐯 for AOPT = 3. D1 D2 D3 Define components of vector 𝐝 for AOPT = 2. Remarks: For the orthotropic definition it is referred to Material Type 2 and 21. *MAT_CELLULAR_RUBBER This is Material Type 87. This material model provides a cellular rubber model with confined air pressure combined with linear viscoelasticity as outlined by Christensen [1980]. See Figure M87-1. Card 1 1 Variable MID 2 RO Type A8 F 3 PR F 4 N I 5 6 7 8 Card 2 if N > 0, a least squares fit is computed from uniaxial data Card 2 1 Variable SGL 2 SW Type F F 3 ST F 4 5 6 7 8 LCID F Card 2 if N = 0, define the following constants Card 2 1 2 3 4 5 6 7 8 Variable C10 C01 C11 C20 C02 Type F Card 3 Variable 1 P0 F 2 PHI F 3 IVS Type F F F VARIABLE MID 6 7 8 F 4 G F F 5 BETA F DESCRIPTION Material identification. A unique number or label not exceeding 8 characters must be specified. RO Mass density VARIABLE DESCRIPTION PR N Poisson’s ratio, typical values are between .0 to .2. Due to the large compressibility of air, large values of Poisson’s ratio generates physically meaningless results. Order of fit (currently < 3). If n > 0 then a least square fit is computed with uniaxial data. The parameters given on card 2 should be specified. Also see *MAT_MOONEY_RIVLIN_RUB- BER (material model 27). A Poisson’s ratio of .5 is assumed for the void free rubber during the fit. The Poisson’s ratio defined on Card 1 is for the cellular rubber. A void fraction formulation is used. Define, if N > 0: SGL SW ST LCID Define, if N = 0: C10 C01 C11 C20 C02 P0 PHI IVS G Specimen gauge length l0 Specimen width Specimen thickness Load curve ID giving the force versus actual change ΔL in the gauge length. If SGL, SW, and ST are set to unity (1.0), then curve LCID is also engineering stress versus engineering strain. Coefficient, C10 Coefficient, C01 Coefficient, C11 Coefficient, C20 Coefficient, C02 Initial air pressure, P0 Ratio of cellular rubber to rubber density, Φ Initial volumetric strain, γ 0 Optional shear relaxation modulus, 𝐺, for rate effects (viscosity) BETA Optional decay constant, 𝛽1 Rubber Block with Entrapped Air Air Figure M87-1. Cellular rubber with entrapped air. By setting the initial air pressure to zero, an open cell, cellular rubber can be simulated. Remarks: Rubber is generally considered to be fully incompressible since the bulk modulus greatly exceeds the shear modulus in magnitude. To model the rubber as an unconstrained material a hydrostatic work term, 𝑊𝐻(𝐽), is included in the strain energy functional which is function of the relative volume, 𝐽, [Ogden 1984]: 𝑊(𝐽1, 𝐽2, 𝐽) = ∑ 𝐶𝑝𝑞(𝐽1 − 3)𝑝 𝑝,𝑞=0 (𝐽2 − 3)𝑞 + 𝑊𝐻(𝐽) 𝐽1 + 𝐼1𝐼3 𝐽2 + 𝐼2𝐼3 −1 3⁄ −2 3⁄ In order to prevent volumetric work from contributing to the hydrostatic work the first and second invariants are modified as shown. This procedure is described in more detail by Sussman and Bathe [1987]. The effects of confined air pressure in its overall response characteristics is included by augmenting the stress state within the element by the air pressure. 𝜎𝑖𝑗 = 𝜎𝑖𝑗 𝑠𝑘 − 𝛿𝑖𝑗𝜎 air 𝑠𝑘 is the bulk skeletal stress and 𝜎 𝑎𝑖𝑟 is the air pressure computed from the where 𝜎𝑖𝑗 equation: 𝜎 air = − 𝑝0𝛾 1 + 𝛾 − 𝜙 where p0 is the initial foam pressure usually taken as the atmospheric pressure and γ defines the volumetric strain 𝛾 = 𝑉 − 1 + 𝛾0 where V is the relative volume of the voids and γ0 is the initial volumetric strain which is typically zero. The rubber skeletal material is assumed to be incompressible. Rate effects are taken into account through linear viscoelasticity by a convolution integral of the form: 𝜎𝑖𝑗 = ∫ 𝑔 𝑖𝑗𝑘𝑙 (𝑡 − 𝜏) ∂𝜀𝑘𝑙 ∂𝜏 𝑑𝜏 or in terms of the second Piola-Kirchhoff stress, 𝑆𝑖𝑗, and Green's strain tensor, 𝐸𝑖𝑗, 𝑆𝑖𝑗 = ∫ 𝐺 𝑖𝑗𝑘𝑙 (𝑡 − 𝜏) ∂𝜀𝑘𝑙 ∂𝜏 𝑑𝜏 (𝑡 − 𝜏) and 𝐺 𝑖𝑗𝑘𝑙 where 𝑔 𝑖𝑗𝑘𝑙 measures. This stress is added to the stress tensor determined from the strain energy functional. (𝑡 − 𝜏)are the relaxation functions for the different stress Since we wish to include only simple rate effects, the relaxation function is represented by one term from the Prony series: 𝑔(𝑡) = 𝛼0 + ∑ 𝛼𝑚𝑒−𝛽𝑡 𝑚=1 given by, 𝑔(𝑡) = 𝐸𝑑𝑒−𝛽1𝑡. This model is effectively a Maxwell fluid which consists of a damper and spring in series. We characterize this in the input by a shear modulus, 𝐺, and decay constant, 𝛽1. The Mooney-Rivlin rubber model (model 27) is obtained by specifying n = 1 without air pressure and viscosity. In spite of the differences in formulations with Model 27, we find that the results obtained with this model are nearly identical with those of material type 27 as long as large values of Poisson’s ratio are used. *MAT_MTS This is Material Type 88. The MTS model is due to Mauldin, Davidson, and Henninger [1990] and is available for applications involving large strains, high pressures and strain rates. As described in the foregoing reference, this model is based on dislocation mechanics and provides a better understanding of the plastic deformation process for ductile materials by using an internal state variable call the mechanical threshold stress. This kinematic quantity tracks the evolution of the material’s microstructure along some arbitrary strain, strain rate, and temperature-dependent path using a differential form that balances dislocation generation and recovery processes. Given a value for the mechanical threshold stress, the flow stress is determined using either a thermal- activation-controlled or a drag-controlled kinetics relationship. An equation-of-state is required for solid elements and a bulk modulus must be defined below for shell elements. Card 1 1 Variable MID Type A8 Card 2 1 2 RO F 2 3 4 5 6 7 8 SIGA SIGI SIGS SIG0 BULK F 3 F 4 F 5 F 6 F 7 8 Variable HF0 HF1 HF2 SIGS0 EDOTS0 BURG CAPA BOLTZ Type F Card 3 1 F 2 F 3 F 4 F 5 F 6 F 7 F 8 Variable SM0 SM1 SM2 EDOT0 GO PINV QINV EDOTI Type F Card 4 1 F 2 F 3 F 4 F 5 F 6 F 7 F 8 Variable G0I PINVI QINVI EDOTS G0S PINVS QINVS Type F F F F F F Card 5 1 2 3 4 5 6 7 8 Variable RHOCPR TEMPRF ALPHA EPS0 Type F F VARIABLE DESCRIPTION MID RO SIGA SIGI SIGS SIG0 HF0 HF1 HF2 SIGS0 BULK Material identification. A unique number or label not exceeding 8 characters must be specified. Mass density 𝜎̂𝑎, dislocation interactions with long-range barriers (force/area). 𝜎̂𝑖, dislocation interactions with interstitial atoms (force/area). 𝜎̂𝑠, dislocation interactions with solute atoms (force/area). 𝜎̂0, initial value of 𝜎̂ at zero plastic strain (force/area) NOT USED. 𝑎0, dislocation generation material constant (force/area). 𝑎1, dislocation generation material constant (force/area). 𝑎2, dislocation generation material constant (force/area). 𝜎̂εso, saturation threshold stress at 0o K (force/area). Bulk modulus defined for shell elements only. Do not input for solid elements. EDOTS0 𝜀̇εso, reference strain-rate (time-1). BURG Magnitude of Burgers vector (distance) (interatomic slip distance), CAPA Material constant, A. BOLTZ Boltzmann’s constant, k (energy/degree). SM0 SM1 𝐺0, shear modulus at zero degrees Kelvin (force/area). 𝑏1, shear modulus constant (force/area). DESCRIPTION *MAT_MTS SM2 𝑏2, shear modulus constant (degree). EDOT0 𝜀̇𝑜, reference strain-rate (time-1). G0 PINV QINV 𝑔0, normalized activation energy for a dislocation/dislocation interaction. 𝑝, material constant. 𝑞, material constant. EDOTI 𝜀̇𝑜,𝑖, reference strain-rate (time-1). G0I PINVI QINVI 𝑔0,𝑖, normalized activation energy for a dislocation/interstitial interaction. 𝑝𝑖 𝑞𝑖 , material constant. , material constant. EDOTS 𝜀̇𝑜,𝑠, reference strain-rate (time-1). G0S PINVS QINVS 𝑔0,𝑠 normalized activation energy for a dislocation/solute interaction. 𝑝𝑠 𝑞𝑠 , material constant. , material constant. RHOCPR 𝜌𝑐𝑝, product of density and specific heat. TEMPRF 𝑇ref, initial element temperature in degrees K. ALPHA 𝛼, material constant (typical value is between 0 and 2). EPS0 𝜀𝑜, factor to normalize strain rate in the calculation of Θ𝑜. (time-1). Remarks: The flow stress 𝜎 is given by: 𝜎 = 𝜎̂𝑎 + 𝐺0 [𝑠th𝜎̂ + 𝑠th,𝑖𝜎̂𝑖 + 𝑠th,𝑠𝜎̂𝑠] The first product in the equation for 𝜏 contains a micro-structure evolution variable, i.e.,𝜎̂ , called the Mechanical Threshold Stress (MTS), that is multiplied by a constant- structure deformation variable s𝑡ℎ: s𝑡ℎ is a function of absolute temperature T and the plastic strain-rates 𝜀̇p. The evolution equation for 𝜎̂ is a differential hardening law representing dislocation-dislocation interactions: ∂ ∂𝜀𝑝 ≡ Θ𝑜 ⎡ ⎢⎢ 1 − ⎢ ⎣ tanh (𝛼 𝜎̂ 𝜎̂𝜀𝑠 tanh(𝛼) ) ⎤ ⎥⎥ ⎥ ⎦ The term, ∂𝜎̂ ∂𝜀𝑝, represents the hardening due to dislocation generation and the stress ratio, 𝜎̂ , represents softening due to dislocation recovery. The threshold stress at zero 𝜎̂𝜀𝑠 strain-hardening 𝜎̂𝜀𝑠 is called the saturation threshold stress. Relationships for Θ𝑜, 𝜎̂𝜀𝑠 are: Θ𝑜 = 𝑎𝑜 + 𝑎1ln ( 𝜀̇𝑝 𝜀0 ) + 𝑎2√ 𝜀̇𝑝 𝜀0 which contains the material constants, 𝑎𝑜, 𝑎1, and 𝑎2. The constant, 𝜎̂𝜀𝑠, is given as: 𝜎̂εs = 𝜎̂εso ( 𝑘𝑇/𝐺𝑏3𝐴 ) 𝜀̇𝑝 𝜀̇εso which contains the input constants: 𝜎̂𝜀𝑠𝑜, 𝜀̇𝜀𝑠𝑜, 𝑏, A, and k. The shear modulus G appearing in these equations is assumed to be a function of temperature and is given by the correlation. 𝐺 = 𝐺0 − 𝑏1 (𝑒𝑏2 𝑇⁄ − 1) ⁄ which contains the constants: 𝐺0, 𝑏1, and 𝑏2. For thermal-activation controlled deformation 𝑠𝑡ℎ is evaluated via an Arrhenius rate equation of the form: ⎧ {{{ ⎨ {{{ ⎩ The absolute temperature is given as: 𝑠𝑡ℎ = 1 − ⎡𝑘𝑇ln ( ⎢⎢⎢ ⎣ 𝐺𝑏3𝑔0 𝜀̇0 𝜀̇𝑝) ⎤ ⎥⎥⎥ ⎦ ⎫ }}} ⎬ }}} ⎭ where E is the internal energy density per unit initial volume. 𝑇 = 𝑇ref + 𝜌𝑐𝑝 *MAT_PLASTICITY_POLYMER This is Material Type 89. An elasto-plastic material with an arbitrary stress versus strain curve and arbitrary strain rate dependency can be defined. It is intended for applications where the elastic and plastic sections of the response are not as clearly distinguishable as they are for metals. Rate dependency of failure strain is included. Many polymers show a more brittle response at high rates of strain. 5 6 7 8 Card 1 1 Variable MID 2 RO Type A8 F 3 E F 4 PR F Default none none none none Card 2 Variable Type Default 1 C F 0 Card 3 1 2 P F 0 2 3 4 5 6 7 8 LCSS LCSR F 0 3 F 0 4 5 6 7 8 Variable EFTX DAMP RFAC LCFAIL Type Default F 0 F 0 F 0 F 0 VARIABLE MID DESCRIPTION Material identification. A unique number or label not exceeding 8 characters must be specified. RO Mass density. VARIABLE DESCRIPTION E PR C P Young’s modulus. Poisson’s ratio. Strain rate parameter, 𝐶, (Cowper Symonds). Strain rate parameter, 𝑃, (Cowper Symonds). LCSS Curve ID or Table ID. 1. Case 1: LCSS is a curve ID. The curve defines effective stress as a function of total effective strain. 2. Case 2: LCSS is a table ID. Each strain rate value in the table is associated to a curve ID giving the stress as a function of effective strain for that rate. The strain rate values defined in the table may be given as the natural logarithm of the strain rate. If the first stress-strain curve in the table corresponds to a negative strain rate, LS-DYNA assumes that the natural logarithm of the strain rate value is used. Since the tables are inter- nally discretized to equally space the points, natural logarithms are necessary, for example, if the curves corre- spond to rates from 10−4 to 104. LCSR Load curve ID defining strain rate scaling effect on yield stress. If LCSR is negative, the load curve is evaluated using a binary search for the correct interval for the strain rate. The binary search is slower than the default incremental search, but in cases where large changes in the strain rate may occur over a single time step, it is more robust. EFTX Failure flag. EQ.0.0: failure determined by maximum tensile strain (default), EQ.1.0: failure determined only by tensile strain in local 𝑥 direction, EQ.2.0: failure determined only by tensile strain in local 𝑦 direction. DAMP Stiffness-proportional damping ratio. Typical values are 10−3 or 10−4. If set too high instabilities can result. Filtering factor for strain rate effects. Must be between 0 (no filtering) and 1 (infinite filtering). The filter is a simple low pass filter to remove high frequency oscillation from the strain rates before they are used in rate effect calculations. The cut off frequency of the filter is [(1 - RFAC) / timestep] rad/sec. Load curve ID giving variation of failure strain with strain rate. The points on the 𝑥-axis should be natural log of strain rate, the 𝑦- axis should be the true strain to failure. Typically this is measured by uniaxial tensile test, and the strain values converted to true strain. *MAT_089 VARIABLE RFAC LCFAIL Remarks: 1. M89 vs. M24. MAT_089 is the same as MAT_024 except for the following points: • Load curve lookup for yield stress is based on equivalent uniaxial strain, not plastic strain (Remarks 2 and 3) • elastic stiffness is initially equal to 𝐸 but will be increased according to the slope of the stress-strain curve (Remark 7) • special strain calculation used for failure and damage (Remark 2) • failure strain depends on strain rate (Remark 4) 2. Strain Calculation for Failure and Damage. The strain used for failure and damage calculation, 𝜀pm is based on an approximation of the greatest value of maximum principal strain encountered during the analysis: 𝜀pm = max i≤n where 𝑛 = current time step index (𝜀𝐻 𝑖 + 𝜀VM ) max 𝑖≤𝑛 (. . . ) = maximum value attained by the argument during the calculation 𝜀𝐻 = 𝜀𝑥 + 𝜀𝑦 + 𝜀𝑧 𝜀𝑥, 𝜀𝑦, 𝜀𝑧 = cumulative strain in the local x, y, or z direction 𝜀vm = √ tr(𝛆′T𝛆′), the usual definition of equivalent uniaxial strain 𝛆′ = deviatoric strain tensor, where each 𝜀𝑥, 𝜀𝑦, and 𝜀𝑧 is cumulative 3. Yield Stress Load Curves. When looking up yield stress from the load curve LCSS, the 𝑥-axis value is 𝜀vm. 4. Failure Strain Load Curves. 𝜀sr = d𝜀pm d𝑡 = strain rate for failure and damage calculation 𝜀𝐹 = LCFAIL(𝜀𝑠𝑟) = Instantanous true strain to failure from look-up on the curve LCFAIL 5. Damage. A damage approach is used to avoid sudden shocks when the failure strain is reached. Damage begins when the "strain ratio," 𝑅, reaches 1.0, where 𝑅 = ∫ 𝑑𝜀pm 𝜀𝐹 . Damage is complete, and the element fails and is deleted, when 𝑅 = 1.1. The damage, 𝐷 = {⎧1.0 ⎩{⎨ 10(1.1 − 𝑅) 1.0 < 𝑅 < 1.1 𝑅 < 1.0 is a reduction factor applied to all stresses, for example, when 𝑅 = 1.05, then 𝐷 = 0.5. 6. Strain Definitions. Unlike other LS-DYNA material models, both the input stress-strain curve and the strain to failure are defined as total true strain, not plastic strain. The input can be defined from uniaxial tensile tests; nominal stress and nominal strain from the tests must be converted to true stress and true strain. The elastic component of strain must not be subtracted out. 7. Elastic Stiffness Scaling. The stress-strain curve is permitted to have sections steeper (i.e. stiffer) than the elastic modulus. When these are encountered the elastic modulus is increased to prevent spurious energy generation. The elastic stiffness is scaled by a factor 𝑓e, which is calculated as follows: 𝑓𝑒 = max (1.0, 𝑠max 3𝐺 ) where 𝐺 = initial shear modulus 𝑆max = maximum slope of stress-strain curve encountered during the analysis 8. Precision. Double precision is recommended when using this material model, especially if the strains become high. 9. Shell Numbering. Invariant shell numbering is recommended when using this material model. See *CONTROL_ACCURACY. *MAT_ACOUSTIC This is Material Type 90. This model is appropriate for tracking low pressure stress waves in an acoustic media such as air or water and can be used only with the acoustic pressure element formulation. The acoustic pressure element requires only one unknown per node. This element is very cost effective. Optionally, cavitation can be allowed. Card 1 1 Variable MID 2 RO Type A8 F Card 2 Variable 1 XP Type F 2 YP F 3 C F 3 ZP F 4 BETA F 4 XN F 5 CF F 5 YN F 6 7 8 ATMOS GRAV F 7 8 F 6 ZN F VARIABLE DESCRIPTION MID RO C Material identification. A unique number or label not exceeding 8 characters must be specified. Mass density Sound speed BETA Damping factor. Recommend values are between 0.1 and 1.0. CF Cavitation flag: EQ.0.0: off, EQ.1.0: on. ATMOS Atmospheric pressure (optional) GRAV Gravitational acceleration constant (optional) XP YP 2-484 (EOS) x-coordinate of free surface point VARIABLE DESCRIPTION ZP XN YN ZN z-coordinate of free surface point x-direction cosine of free surface normal vector y-direction cosine of free surface normal vector z-direction cosine of free surface normal vector *MAT_091-092 *MAT_SOFT_TISSUE_{OPTION} Available options include: <BLANK> VISCO *MAT_SOFT_TISSUE This is Material Type 91 (OPTION=<BLANK>) or Material Type 92 (OPTION = VISCO). This material is a transversely isotropic hyperelastic model for representing biological soft tissues such as ligaments, tendons, and fascia. The representation provides an isotropic Mooney-Rivlin matrix reinforced by fibers having a strain energy contribution with the qualitative material behavior of collagen. The model has a viscoelasticity option which activates a six-term Prony series kernel for the relaxation function. In this case, the hyperelastic strain energy represents the elastic (long-time) response. See Weiss et al. [1996] and Puso and Weiss [1998] for additional details. NOTE: This material does not support specification of a ma- terial angle, 𝛽𝑖, for each through-thickness integra- tion point of a shell. Card 1 1 Variable MID Type A8 Card 2 Variable 1 XK 2 RO F 2 3 C1 F 3 4 C2 F 4 5 C3 F 5 6 C4 F 6 7 C5 F 7 XLAM FANG XLAM0 FAILSF FAILSM FAILSHR Type F F F F F F F Card 3 1 Variable AOPT Type F 2 AX F 3 AY F 4 AZ F 5 BX F 6 BY F 7 BZ F 8 8 Card 4 1 2 3 4 5 6 7 8 Variable LA1 LA2 LA3 MACF Type F F F I Prony Series Card 1. Additional card for VISCO keyword option. Card 5 Variable 1 S1 Type F 2 S2 F 3 S3 F 4 S4 F 5 S5 F 6 S6 F Prony Series Card 2. Additional card for VISCO keyword option. Card 6 Variable 1 T1 Type F 2 T2 F 3 T3 F 4 T4 F 5 T5 F 6 T6 F 7 8 7 8 VARIABLE MID DESCRIPTION Material identification. exceeding 8 characters must be specified. A unique number or label not RO Mass density C1 - C5 Hyperelastic coefficients XK Bulk Modulus XLAM FANG Stretch ratio at which fibers are straightened Fiber angle in local shell coordinate system (shells only) XLAM0 Initial fiber stretch (optional) FAILSF Stretch ratio for ligament fibers at failure (applies to shell elements only). If zero, failure is not considered. VARIABLE FAILSM FAILSHR DESCRIPTION Stretch ratio for surrounding matrix material at failure (applies to shell elements only). If zero, failure is not considered. Shear strain at failure at a material point (applies to shell elements only). If zero, failure is not considered. This failure value is independent of FAILSF and FAILSM. AOPT Material axes option, see Figure M2-1 (bricks only): EQ.0.0: locally orthotropic with material axes determined by element nodes as shown in Figure M2-1. Nodes 1, 2, and 4 of an element are identical to the nodes used for the definition of a coordinate system as by *DE- FINE_COORDINATE_NODES. EQ.1.0: locally orthotropic with material axes determined by a point in space and the global location of the ele- ment center; this is the 𝑎-direction. This option is for solid elements only. EQ.2.0: globally orthotropic with material axes determined by vectors defined below, as with *DEFINE_COOR- DINATE_VECTOR. EQ.3.0: locally orthotropic material axes determined by a line in the plane of the element defined by the cross product of the vector 𝐯 with the element normal. The plane of a solid element is the midsurface be- tween the inner surface and outer surface defined by the first four nodes and the last four nodes of the connectivity of the element, respectively. EQ.4.0: locally orthotropic in cylindrical coordinate system with the material axes determined by a vector 𝐯, and an originating point, 𝐩, which define the centerline axis. This option is for solid elements only. LT.0.0: the absolute value of AOPT is a coordinate system ID number (CID on *DEFINE_COORDINATE_- or NODES, *DEFINE_COORDINATE_VECTOR). Available in R3 version of 971 and later. *DEFINE_COORDINATE_SYSTEM AX, AY, AZ Equal to XP, YP, ZP for AOPT = 1, Equal to A1, A2, A3 for AOPT = 2, Equal to V1, V2, V3 for AOPT = 3 or 4. VARIABLE BX, BY, BZ DESCRIPTION Equal to D1, D2, D3 for AOPT = 2 Equal to XP, YP, ZP for AOPT = 4 LAX, LAY, LAZ Local fiber orientation vector (bricks only) MACF Material axes change flag for brick elements: EQ.1: No change, default, EQ.2: switch material axes 𝑎 and 𝑏, EQ.3: switch material axes 𝑎 and 𝑐, EQ.4: switch material axes 𝑏 and 𝑐. Factors in the Prony series. Characteristic times for Prony series relaxation kernel for VISCO option. S1 – S6 T1 - T6 Remarks: The overall strain energy 𝑊 is "uncoupled" and includes two isotropic deviatoric matrix terms, a fiber term 𝐹, and a bulk term: 𝑊 = 𝐶1(𝐼 ̃1 − 3) + 𝐶2(𝐼 ̃2 − 3) + 𝐹(𝜆) + 𝐾[ln(𝐽)]2 Here, 𝐼 ̃1 and 𝐼 ̃2 are the deviatoric invariants of the right Cauchy deformation tensor, 𝜆 is the deviatoric part of the stretch along the current fiber direction, and 𝐽 = det𝐅 is the volume ratio. The material coefficients 𝐶1 and 𝐶2 are the Mooney-Rivlin coefficients, while K is the effective bulk modulus of the material (input parameter XK). The derivatives of the fiber term 𝐹 are defined to capture the behavior of crimped collagen. The fibers are assumed to be unable to resist compressive loading - thus the model is isotropic when 𝜆 < 1. An exponential function describes the straightening of the fibers, while a linear function describes the behavior of the fibers once they are straightened past a critical fiber stretch level 𝜆 ≥ 𝜆∗ (input parameter XLAM): ∂𝐹 ∂𝜆 = ⎧ {{{{ {{{{ ⎨ ⎩ 𝐶3 𝜆 < 1 [exp(𝐶4(𝜆 − 1)) − 1] 𝜆 < 𝜆∗ (𝐶5𝜆 + 𝐶6) 𝜆 ≥ 𝜆∗ Coefficients 𝐶3, 𝐶4, and 𝐶5 must be defined by the user. 𝐶6 is determined by LS-DYNA to ensure stress continuity at 𝜆 = 𝜆∗. Sample values for the material coefficients 𝐶1 − 𝐶5 and 𝜆∗ for ligament tissue can be found in Quapp and Weiss [1998]. The bulk modulus 𝐾 should be at least 3 orders of magnitude larger than 𝐶1 to ensure near-incompressible material behavior. Viscoelasticity is included via a convolution integral representation for the time- dependent second Piola-Kirchoff stress 𝐒(𝐂, 𝑡): 𝐒(𝐂, 𝑡) = 𝐒𝑒(𝐂) + ∫ 2𝐺(𝑡 − 𝑠) 𝜕𝑊 𝜕𝐂(𝑠) 𝑑𝑠 Here, 𝐒𝑒 is the elastic part of the second PK stress as derived from the strain energy, and 𝐺(𝑡 − 𝑠) is the reduced relaxation function, represented by a Prony series: 𝐺(𝑡) = ∑ 𝑆𝑖exp ( 𝑖=1 𝑇𝑖 ) Puso and Weiss [1998] describe a graphical method to fit the Prony series coefficients to relaxation data that approximates the behavior of the continuous relaxation function proposed by Y-C. Fung, as quasilinear viscoelasticity. Remarks on Input Parameters: Cards 1 through 4 must be included for both shell and brick elements, although for shells cards 3 and 4 are ignored and may be blank lines. For shell elements, the fiber direction lies in the plane of the element. The local axis is defined by a vector between nodes n1 and n2, and the fiber direction may be offset from this axis by an angle FANG. For brick elements, the local coordinate system is defined using the convention described previously for *MAT_ORTHOTROPIC_ELASTIC. The fiber direction is oriented in the local system using input parameters LAX, LAY, and LAZ. By default, (LAX, LAY, LAZ) = (1,0,0) and the fiber is aligned with the local x-direction. An optional initial fiber stretch can be specified using XLAM0. The initial stretch is applied during the first time step. This creates preload in the model as soft tissue contacts and equilibrium is established. For example, a ligament tissue "uncrimping strain" of 3% can be represented with initial stretch value of 1.03. If the VISCO option is selected, at least one Prony series term (S1, T1) must be defined. *MAT_ELASTIC_6DOF_SPRING_DISCRETE_BEAM This is Material Type 93. This material model is defined for simulating the effects of nonlinear elastic and nonlinear viscous beams by using six springs each acting about one of the six local degrees-of-freedom. The input consists of part ID's that reference material type, *MAT_ELASTIC_SPRING_DISCRETE_BEAM above (type 74 above). Generally, these referenced parts are used only for the definition of this material model and are not referenced by any elements. The two nodes defining a beam may be coincident to give a zero length beam, or offset to give a finite length beam. For finite length discrete beams the absolute value of the variable SCOOR in the SECTION_- BEAM input should be set to a value of 2.0, which causes the local r-axis to be aligned along the two nodes of the beam to give physically correct behavior. The distance between the nodes of a beam should not affect the behavior of this material model. A triad is used to orient the beam for the directional springs. Card 1 1 Variable MID 2 RO 3 4 5 6 7 8 TPIDR TPIDS TPIDT RPIDR RPIDS RPIDT Type A8 F I I I I I I VARIABLE MID DESCRIPTION Material identification. A unique number or label not exceeding 8 characters must be specified. RO Mass density, see also volume in *SECTION_BEAM definition. TPIDR TPIDS TPIDT RPIDR RPIDS Translational motion in the local r-direction is governed by part ID TPIDR. If zero, no force is computed in this direction. Translational motion in the local s-direction is governed by part ID TPIDS. If zero, no force is computed in this direction. Translational motion in the local t-direction is governed by part ID TPIDT. If zero, no force is computed in this direction. Rotational motion about the local r-axis is governed by part ID RPIDR. If zero, no moment is computed about this axis. Rotational motion about the local s-axis is governed by part ID RPIDS. If zero, no moment is computed about this axis. RPIDT *MAT_ELASTIC_6DOF_SPRING_DISCRETE_BEAM DESCRIPTION Rotational motion about the local t-axis is governed by part ID RPIDT. If zero, no moment is computed about this axis. *MAT_INELASTIC_SPRING_DISCRETE_BEAM This is Material Type 94. This model permits elastoplastic springs with damping to be represented with a discrete beam element type 6. A yield force versus deflection curve is used which can vary in tension and compression. Card 1 1 Variable MID Type A8 Card 2 1 2 RO F 2 Variable FLCID HLCID Type F F 3 K F 3 C1 F 4 F0 F 4 C2 F 5 D F 5 6 7 8 CDF TDF F 6 F 7 8 DLE GLCID F I VARIABLE DESCRIPTION MID RO K F0 D CDF TDF Material identification. A unique number or label not exceeding 8 characters must be specified. Mass density, see also volume in *SECTION_BEAM definition. Elastic loading/unloading stiffness. This is required input. Optional initial force. This option is inactive if this material is referenced in a part referenced by material type *MAT_INELAS- TIC_6DOF_SPRING Optional viscous damping coefficient. Compressive displacement at failure. Input as a positive number. After failure, no forces are carried. This option does not apply to zero length springs. EQ.0.0: inactive. Tensile displacement at failure. After failure, no forces are carried. EQ.0.0: inactive. FLCID *MAT_INELASTIC_SPRING_DISCRETE_BEAM DESCRIPTION Load curve ID, see *DEFINE_CURVE, defining the yield force versus plastic deflection. If the origin of the curve is at (0,0) the force magnitude is identical in tension and compression, i.e., only the sign changes. If not, the yield stress in the compression is used when the spring force is negative. The plastic displacement increases monotonically in this implementation. The load curve is required input. HLCID Load curve ID, see *DEFINE_CURVE, defining force versus relative velocity (Optional). If the origin of the curve is at (0,0) the force magnitude is identical for a given magnitude of the relative velocity, i.e., only the sign changes. C1 C2 Damping coefficient. Damping coefficient DLE Factor to scale time units. GLCID Optional load curve ID, see *DEFINE_CURVE, defining a scale factor versus deflection for load curve ID, HLCID. If zero, a scale factor of unity is assumed. Remarks: The yield force is taken from the load curve: 𝐹𝑌 = 𝐹𝑦(Δ𝐿plastic) where 𝐿plastic is the plastic deflection. A trial force is computed as: and is checked against the yield force to determine 𝐹: 𝐹𝑇 = 𝐹𝑛 + K × Δ𝐿̇(Δ𝑡) 𝐹 = { 𝐹𝑌 𝑖𝑓 𝐹𝑇 > 𝐹𝑌 𝐹𝑇 𝑖𝑓 𝐹𝑇 ≤ 𝐹𝑌 The final force, which includes rate effects and damping, is given by: 𝐹𝑛+1 = 𝐹 × [1 + C1 × Δ𝐿̇ + C2 × sgn(Δ𝐿̇)ln (max {1. , ∣Δ𝐿̇∣ DLE })] + D×Δ𝐿̇ + 𝑔(Δ𝐿)ℎ(Δ𝐿̇) Unless the origin of the curve starts at (0,0), the negative part of the curve is used when the spring force is negative where the negative of the plastic displacement is used to interpolate, 𝐹𝑦. The positive part of the curve is used whenever the force is positive. In these equations, Δ𝐿 is the change in length Δ𝐿 = current length - initial length The cross sectional area is defined on the section card for the discrete beam elements, See *SECTION_BEAM. The square root of this area is used as the contact thickness offset if these elements are included in the contact treatment. *MAT_INELASTIC_6DOF_SPRING_DISCRETE_BEAM type, *MAT_INELASTIC_SPRING_DISCRETE_BEAM above This is Material Type 95. This material model is defined for simulating the effects of nonlinear inelastic and nonlinear viscous beams by using six springs each acting about one of the six local degrees-of-freedom. The input consists of part ID's that reference material (type 94). Generally, these referenced parts are used only for the definition of this material model and are not referenced by any elements. The two nodes defining a beam may be coincident to give a zero length beam, or offset to give a finite length beam. For finite length discrete beams the absolute value of the variable SCOOR in the SECTION_- BEAM input should be set to a value of 2.0, which causes the local r-axis to be aligned along the two nodes of the beam to give physically correct behavior. The distance between the nodes of a beam should not affect the behavior of this material model. A triad must be used to orient the beam for zero length beams. Card 1 1 Variable MID 2 RO 3 4 5 6 7 8 TPIDR TPIDS TPIDT RPIDR RPIDS RPIDT Type A8 F I I I I I I VARIABLE MID DESCRIPTION Material identification. A unique number or label not exceeding 8 characters must be specified. RO Mass density, see also volume in *SECTION_BEAM definition. TPIDR TPIDS TPIDT RPIDR RPIDS Translational motion in the local r-direction is governed by part ID TPIDR. If zero, no force is computed in this direction. Translational motion in the local s-direction is governed by part ID TPIDS. If zero, no force is computed in this direction. Translational motion in the local t-direction is governed by part ID TPIDT. If zero, no force is computed in this direction. Rotational motion about the local r-axis is governed by part ID RPIDR. If zero, no moment is computed about this axis. Rotational motion about the local s-axis is governed by part ID RPIDS. If zero, no moment is computed about this axis. VARIABLE RPIDT DESCRIPTION Rotational motion about the local t-axis is governed by part ID RPIDT. If zero, no moment is computed about this axis. This is Material Type 96. Card 1 1 Variable MID Type A8 Card 2 1 2 RO F 2 *MAT_BRITTLE_DAMAGE 3 E F 3 4 PR F 4 5 6 7 8 TLIMIT SLIMIT FTOUGH SRETEN F 5 F 6 F 7 F 8 Variable VISC FRA_RF E_RF YS_RF EH_RF FS_RF SIGY Type F F F F F F F VARIABLE DESCRIPTION MID RO E PR Material identification. A unique number or label not exceeding 8 characters must be specified. Mass density. Young's modulus. Poisson's ratio. TLIMIT Tensile limit. SLIMIT Shear limit. FTOUGH Fracture toughness. SRETEN Shear retention. VISC Viscosity. FRA_RF Fraction of reinforcement in section. E_RF Young's modulus of reinforcement. YS_RF Yield stress of reinforcement. EH_RF Hardening modulus of reinforcement. VARIABLE DESCRIPTION Failure strain (true) of reinforcement. Compressive yield stress. EQ.0: no compressive yield FS_RF SIGY Remarks: A full description of the tensile and shear damage parts of this material model is given in Govindjee, Kay and Simo [1994,1995]. It is an anisotropic brittle damage model designed primarily for concrete though it can be applied to a wide variety of brittle materials. It admits progressive degradation of tensile and shear strengths across smeared cracks that are initiated under tensile loadings. Compressive failure is governed by a simplistic J2 flow correction that can be disabled if not desired. Damage is handled by treating the rank 4 elastic stiffness tensor as an evolving internal variable for the material. Softening induced mesh dependencies are handled by a characteristic length method [Oliver 1989]. Description of properties: 1. E is the Young's modulus of the undamaged material also known as the virgin modulus. 2. υ is the Poisson's ratio of the undamaged material also known as the virgin Poisson's ratio. 3. 𝑓𝑛 is the initial principal tensile strength (stress) of the material. Once this stress has been reached at a point in the body a smeared crack is initiated there with a normal that is co-linear with the 1st principal direction. Once initiated, the crack is fixed at that location, though it will convect with the motion of the body. As the loading progresses the allowed tensile traction normal to the crack plane is progressively degraded to a small machine dependent constant. The degradation is implemented by reducing the material's modulus normal to the smeared crack plane according to a maximum dissipation law that incorpo- rates exponential softening. The restriction on the normal tractions is given by 𝜙𝑡 = (𝐧 ⊗ 𝐧): σ − 𝑓𝑛 + (1 − 𝜀)𝑓𝑛(1 − exp[−𝐻𝛼]) ≤ 0 where 𝐧 is the smeared crack normal, 𝜀 is the small constant, 𝐻 is the softening modulus, and 𝛼 is an internal variable. 𝐻 is set automatically by the program; see 𝑔𝑐 below. 𝛼 measures the crack field intensity and is output in the equiva- lent plastic strain field, 𝜀̅𝑝, in a normalized fashion. The evolution of alpha is governed by a maximum dissipation argument. When the normalized value reaches unity it means that the material's strength has been reduced to 2% of its original value in the normal and parallel direc- tions to the smeared crack. Note that for plotting purposes it is never output greater than 5. 4. 𝑓𝑠 is the initial shear traction that may be transmitted across a smeared crack plane. The shear traction is limited to be less than or equal to 𝑓𝑠(1 − 𝛽)(1 − exp[−𝐻𝛼]), through the use of two orthogonal shear damage surfaces. Note that the shear degradation is coupled to the tensile degradation through the internal variable alpha which measures the intensity of the crack field. 𝛽 is the shear retention factor defined below. The shear degradation is taken care of by reducing the material's shear stiffness parallel to the smeared crack plane. 5. 𝑔𝑐 is the fracture toughness of the material. It should be entered as fracture energy per unit area crack advance. Once entered the softening modulus is automatically calculated based on element and crack geometries. 6. 𝛽 is the shear retention factor. As the damage progresses the shear tractions allowed across the smeared crack plane asymptote to the product 𝛽𝑓𝑠. 7. 𝜂 represents the viscosity of the material. Viscous behavior is implemented as a simple Perzyna regularization method. This allows for the inclusion of first order rate effects. The use of some viscosity is recommend as it serves as regu- larizing parameter that increases the stability of calculations. 8. 𝜎𝑦 is a uniaxial compressive yield stress. A check on compressive stresses is made using the J2 yield function 𝐬: 𝐬 − √2 3 𝜎𝑦 ≤ 0, where 𝐬 is the stress deviator. If violated, a J2 return mapping correction is executed. This check is executed when (1) no damage has taken place at an integration point yet, (2) when dam- age has taken place at a point but the crack is currently closed, and (3) during active damage after the damage integration (i.e. as an operator split). Note that if the crack is open the plasticity correction is done in the plane-stress subspace of the crack plane. A variety of experimental data has been replicated using this model from quasi-static to explosive situations. Reasonable properties for a standard grade concrete would be E = 3.15x106 psi, 𝑓𝑛 = 450 psi, 𝑓𝑠 = 2100 psi, 𝜈 = 0.2, 𝑔𝑐 = 0.8 lbs/in, 𝛽 = 0.03, 𝜂 = 0.0 psi- sec, 𝜎𝑦 = 4200 psi. For stability, values of 𝜂 between 104 to 106 psi/sec are recommend- ed. Our limited experience thus far has shown that many problems require nonzero values of 𝜂 to run to avoid error terminations. Various other internal variables such as crack orientations and degraded stiffness tensors are internally calculated but currently not available for output. *MAT_GENERAL_JOINT_DISCRETE_BEAM This is Material Type 97. This model is used to define a general joint constraining any combination of degrees of freedom between two nodes. The nodes may belong to rigid or deformable bodies. In most applications the end nodes of the beam are coincident and the local coordinate system (r,s,t axes) is defined by CID . Card 1 1 Variable MID 2 RO Type A8 F 3 TR I 4 TS I 5 TT I 6 RR I 7 RS I 8 RT Remarks 1 Card 2 1 2 3 4 5 6 7 8 Variable RPST RPSR Type Remarks F 2 F VARIABLE DESCRIPTION MID RO TR TS Material identification. A unique number or label not exceeding 8 characters must be specified. Mass density, see also volume in *SECTION_BEAM definition. Translational constraint code along the r-axis (0 ⇒ free, 1 ⇒ constrained) Translational constraint code along the s-axis (0 ⇒ free, 1 ⇒ constrained) *MAT_GENERAL_JOINT_DISCRETE_BEAM DESCRIPTION TT RR RS RT RPST RPSR Remarks: Translational constraint code along the t-axis (0 ⇒ free, 1 ⇒ constrained) Rotational constraint code about the r-axis (0 ⇒ free, 1 ⇒ constrained) Rotational constraint code about the s-axis (0 ⇒ free, 1 ⇒ constrained) Rotational constraint code about the t-axis (0 ⇒ free, 1 ⇒ constrained) Penalty stiffness scale factor for translational constraints. Penalty stiffness scale factor for rotational constraints. 1. For explicit calculations, the additional stiffness due to this joint may require addition mass and inertia for stability. Mass and rotary inertia for this beam element is based on the defined mass density, the volume, and the mass mo- ment of inertia defined in the *SECTION_BEAM input. 2. The penalty stiffness applies to explicit calculations. For implicit calculations, constraint equations are generated and imposed on the system equations; there- fore, these constants, RPST and RPSR, are not used. *MAT_SIMPLIFIED_JOHNSON_COOK_{OPTION} Available options include: <BLANK> STOCHASTIC This is Material Type 98 implementing Johnson/Cook strain sensitive plasticity. It is used for problems where the strain rates vary over a large range. In contrast to the full Johnson/Cook model (material type 15) this model introduces the following simplifications: 1. 2. thermal effects and damage are ignored, and the maximum stress is directly limited since thermal softening which is very significant in reducing the yield stress under adiabatic loading is not available. An iterative plane stress update is used for the shell elements, but due to the simplifications related to thermal softening and damage, this model is 50% faster than the full Johnson/Cook implementation. To compensate for the lack of thermal softening, limiting stress values are introduced to keep the stresses within reasonable limits. A resultant formulation for the Belytschko-Tsay, the C0 Triangle, and the fully integrated type 16 shell elements is available and can be activated by specifying either zero or one through thickness integration point on the *SECTION_SHELL card. While less accurate than through thickness integration, this formulation runs somewhat faster. Since the stresses are not computed in the resultant formulation, the stresses written to the databases for the resultant elements are set to zero. This model is also available for the Hughes-Liu beam, the Belytschko-Schwer beam, and for the truss element. For the resultant beam formulation, the rate effects are approximated by the axial rate, since the thickness of the beam about it bending axes is unknown. Because this model is primarily used for structural analysis, the pressure is determined using the linear bulk modulus. Card 1 1 Variable MID 2 RO Type A8 F 3 E F 4 PR F 5 VP F Default none none none none 0.0 6 7 8 Card 2 Variable Type 1 A F 2 B F 3 N F 4 C F 5 6 7 8 PSFAIL SIGMAX SIGSAT EPSO F F F F Default none 0.0 0.0 0.0 1.0E+17 SIGSAT 1.0E+28 1.0 VARIABLE DESCRIPTION MID RO E PR VP A B N C Material identification. A unique number or label not exceeding 8 characters must be specified. Mass density Young’s modulus Poisson’s ratio Formulation for rate effects: EQ.0.0: Scale yield stress (default), EQ.1.0: Viscoplastic formulation. This option applies only to the 4-node shell and 8-node thick shell if and only if through thickness integration is used. See equations below. See equations below. See equations below. See equations below. VARIABLE DESCRIPTION PSFAIL Effective plastic strain at failure. If zero failure is not considered. Maximum stress obtainable from work hardening before rate effects are added (optional). This option is ignored if VP = 1.0 Saturation stress which limits the maximum value of effective stress which can develop after rate effects are added (optional). Quasi-static threshold strain rate. See description under *MAT_- 015. SIGMAX SIGSAT EPS0 Remarks: Johnson and Cook express the flow stress as 𝜎𝑦 = (𝐴 + 𝐵𝜀̅ 𝑝𝑛 )(1 + 𝐶 ln 𝜀∗̇ ) where 𝐴, 𝐵, 𝐶 = input constants 𝜀̅𝑝 = effective plastic strain 𝜀∗̇ = 𝜀̅ EPS0 = normalized effective strain rate The maximum stress is limited by SIGMAX and SIGSAT by: 𝜎𝑦 = min{min[𝐴 + 𝐵𝜀̅ 𝑝𝑛 , SIGMAX](1 + 𝑐 ln 𝜀∗̇ ), SIGSAT} Failure occurs when the effective plastic strain exceeds PSFAIL. If the viscoplastic option is active, VP = 1.0, the parameters SIGMAX and SIGSAT are ignored since these parameters make convergence of the viscoplastic strain iteration loop difficult to achieve. The viscoplastic option replaces the plastic strain in the forgoing equations by the viscoplastic strain and the strain rate by the viscoplastic strain rate. Numerical noise is substantially reduced by the viscoplastic formulation. The STOCHASTIC option allows spatially varying yield and failure behavior. See *DE- FINE_STOCHASTIC_VARIATION for additional information. LS-DYNA R10.0 *MAT_SIMPLIFIED_JOHNSON_COOK_ORTHOTROPIC_DAMAGE This is Material Type 99. This model, which is implemented with multiple through thickness integration points, is an extension of model 98 to include orthotropic damage as a means of treating failure in aluminum panels. Directional damage begins after a defined failure strain is reached in tension and continues to evolve until a tensile rupture strain is reached in either one of the two orthogonal directions. After rupture is detected at NUMINT integration points, the element is deleted. Card 1 1 Variable MID 2 RO Type A8 F 3 E F 4 PR F 5 VP F 6 7 8 EPPFR LCDM NUMINT F I I Default none none none none 0.0 1.e+16 optional all points Card 2 Variable Type 1 A F 2 B F 3 N F 4 C F 5 6 7 8 PSFAIL SIGMAX SIGSAT EPSO F F F F Default none 0.0 0.0 0.0 1.0E+17 SIGSAT 1.0E+28 1.0 VARIABLE DESCRIPTION MID RO E PR Material identification. A unique number or label not exceeding 8 characters must be specified. Mass density Young’s modulus Poisson’s ratio *MAT_SIMPLIFIED_JOHNSON_COOK_ORTHOTROPIC_DAMAGE *MAT_099 VARIABLE DESCRIPTION VP Formulation for rate effects: EQ.0.0: Scale yield stress (default), EQ.1.0: Viscoplastic formulation. EPPFR LCDM NUMINT This option applies only to the 4-node shell and 8-node thick shell if and only if through thickness integration is used. Plastic strain at which material ruptures (logarithmic). Load curve ID defining nonlinear damage curve. See Figure M81-2. Number of through thickness integration points which must fail before the element is deleted. (If zero, all points must fail.) The default of all integration points is not recommended since elements undergoing large strain are often not deleted due to nodal fiber rotations which limit 0strains at active integration points after most points have failed. Better results are obtained if NUMINT is set to 1 or a number less than one half of the number of through thickness points. For example, if four through thickness points are used, NUMINT should not exceed 2, even for fully integrated shells which have 16 integration points. A B N C See equations below. See equations below. See equations below. See equations below. PSFAIL Principal plastic strain at failure. If zero failure is not considered. SIGMAX SIGSAT EPS0 Maximum stress obtainable from work hardening before rate effects are added (optional). This option is ignored if VP = 1.0 Saturation stress which limits the maximum value of effective stress which can develop after rate effects are added (optional). Quasi-static threshold strain rate. See description under *MAT_- 015. *MAT_SIMPLIFIED_JOHNSON_COOK_ORTHOTROPIC_DAMAGE See the description for the SIMPLIFIED_JOHNSON_COOK model above. *MAT_100 This is Material Type 100. The material model applies to beam element type 9 and to solid element type 1. The failure models apply to both beam and solid elements. In the case of solid elements, if hourglass type 4 is specified then hourglass type 4 will be used, otherwise, hourglass type 6 will be automatically assigned. Hourglass type 6 is preferred. The beam elements, based on the Hughes-Liu beam formulation, may be placed between any two deformable shell surfaces and tied with constraint contact, *CON- TACT_SPOTWELD, which eliminates the need to have adjacent nodes at spot weld locations. Beam spot welds may be placed between rigid bodies and rigid/deformable bodies by making the node on one end of the spot weld a rigid body node which can be an extra node for the rigid body, see *CONSTRAINED_EXTRA_NODES_OPTION. In the same way rigid bodies may also be tied together with this spot weld option. This weld option should not be used with rigid body switching. The foregoing advice is valid if solid element spot welds are used; however, since the solid elements have just three degrees-of-freedom at each node, *CONTACT_TIED_SURFACE_TO_SURFACE must be used instead of *CONTACT_SPOTWELD. In flat topologies the shell elements have an unconstrained drilling degree-of-freedom which prevents torsional forces from being transmitted. If the torsional forces are deemed to be important, brick elements should be used to model the spot welds. Beam and solid element force resultants for MAT_SPOTWELD are written to the spot weld force file, swforc, and the file for element stresses and resultants for designated elements, elout. It is advisable to include all spot welds, which provide the slave nodes, and spot welded materials, which define the master segments, within a single *CONTACT_- SPOTWELD interface for beam element spot welds or a *CONTACT_TIED_SUR- FACE_TO_SURFACE interface for solid element spot welds. As a constraint method these interfaces are treated independently which can lead to significant problems if such interfaces share common nodal points. An added benefit is that memory usage can be substantially less with a single interface. Available options include: <BLANK> DAMAGE-FAILURE The DAMAGE-FAILURE option causes one additional line to be read with the damage parameter and a flag that determines how failure is computed from the resultants. On this line the parameter, RS, if nonzero, invokes damage mechanics combined with the plasticity model to achieve a smooth drop off of the resultant forces prior to the removal of the spot weld. The parameter OPT determines the method used in computing resultant based failure, which is unrelated to damage. Card 1 1 Variable MID 2 RO Type A8 F 3 E F 4 PR F 5 SIGY F 6 EH F 7 DT F Card 2 for no failure. Additional card for <blank> keyword option. Card 2 1 2 3 4 5 6 7 Variable EFAIL NRR NRS NRT MRR MSS MTT Type F F F F F F F 8 TFAIL F 8 NF F Card 2 for resultant based failure. Additional card for DAMAGE-FAILURE keyword option with OPT = -1.0 or 0.0. Card 2 1 2 3 4 5 6 7 Variable EFAIL NRR NRS NRT MRR MSS MTT Type F F F F F F F 8 NF F Card 2 for stress based failure. Additional card for DAMAGE-FAILURE keyword option with OPT = 1.0 and positive values in fields 2 and 3. Card 2 1 2 3 4 5 6 7 Variable EFAIL SIGAX SIGTAU Type F F F 8 NF Card 2 for stress based failure. Additional card for DAMAGE-FAILURE keyword option with OPT = 1.0 and negative values in fields 2 and 3. Card 2 1 2 3 4 5 6 7 Variable EFAIL -LCAX -LCTAU Type F F F 8 NF F Card 2 for user subroutine based failure. Additional card for DAMAGE-FAILURE keyword option with OPT = 2.0, 12, or 22. Card 2 1 2 3 4 5 6 7 Variable EFAIL USRV1 USRV2 USRV3 USRV4 USRV5 USRV6 Type F F F F F F F Card 2 for OPT = 3.0 or 4.0. Card 2 1 Variable EFAIL Type F Card 2 for OPT = 5.0. Card 2 1 Variable EFAIL Type F 2 ZD F 2 ZD F 3 ZT F 3 ZT F 4 5 6 7 ZALP1 ZALP2 ZALP3 ZRRAD F F F F 5 6 7 8 4 ZT2 F 8 NF F 8 NF Card 2 for OPT = 6.0, 7.0, 9.0, or 10.0. Card 2 1 2 3 4 5 6 7 Variable EFAIL Type F Card 2 for OPT = 11.0. Card 2 1 2 3 4 5 6 7 Variable EFAIL LCT LCC Type F F F 8 NF F 8 NF F Additional card for the DAMAGE-FAILURE option. Card 3 Variable 1 RS 2 3 4 5 6 7 8 OPT FVAL TRUE_T ASFF BETA DMGOPT Type F F F F I F F Optional 2nd additional card for the DAMAGE-FAILURE option, read only if DMGOPT = -1 on card 3. Card 3A 1 2 3 4 5 6 7 8 Variable DMGOPT FMODE FFCAP Type F F F Additional card for OPT = 12 or 22. Card 4 1 2 3 4 5 6 7 8 Variable USRV7 USRV8 USRV9 USRV10 USRV11 USRV12 USRV13 USRV14 Type F F F F F F F Additional card for OPT = 12 or 22 Card 5 1 2 3 4 5 6 7 8 Variable USRV15 USRV16 USRV17 USRV18 USRV19 USRV20 USRV21 USRV22 Type F F F F F F F F VARIABLE DESCRIPTION MID RO E PR SIGY EH DT TFAIL EFAIL NRR NRS Material identification. A unique number or label not exceeding 8 characters must be specified. Mass density Young’s modulus. If input as negative, a uniaxial option for solid spot welds is invoked; see “Uniaxial option” in remarks. Poisson’s ratio GT.0: Initial yield stress. LT.0: A yield curve or table is assigned by |SIGY|. Plastic hardening modulus, 𝐸ℎ Time step size for mass scaling, Δ𝑡 Failure time if nonzero. If zero this option is ignored. Effective plastic strain in weld material at failure. If the damage option is inactive, the spot weld element is deleted when the plastic strain at each integration point exceeds EFAIL. If the damage option is active, the plastic strain must exceed the rupture strain (RS) at each integration point before deletion occurs. 𝐹 at failure Axial force resultant 𝑁𝑟𝑟𝐹 or maximum axial stress 𝜎𝑟𝑟 depending on the value of OPT . If zero, failure due to this component is not considered. If negative, |NRR| is the load curve ID defining the maximum axial stress at failure as a function of the effective strain rate. Force resultant 𝑁𝑟𝑠𝐹 or maximum shear stress 𝜏𝐹 at failure depending on the value of OPT . If zero, failure due to this component is not considered. If negative, |NRS| is the load VARIABLE DESCRIPTION NRT MRR MSS MTT curve ID defining the maximum shear stress at failure as a function of the effective strain rate. Force resultant 𝑁𝑟𝑡𝐹 at failure. If zero, failure due to this component is not considered. Torsional moment resultant 𝑀𝑟𝑟𝐹 at failure. If zero, failure due to this component is not considered. Moment resultant 𝑀𝑠𝑠𝐹 at failure. If zero, failure due to this component is not considered. Moment resultant 𝑀𝑡𝑡𝐹 at failure. If zero, failure due to this component is not considered. NF Number of force vectors stored for filtering. SIGAX SIGTAU LCAX LCTAU Maximum axial stress 𝜎𝑟𝑟 component is not considered. 𝐹 at failure. If zero, failure due to this Maximum shear stress 𝜏𝐹 at failure. If zero, failure due to this component is not considered. Load curve ID defining the maximum axial stress at failure as a function of the effective strain rate. Input as a negative number. Load curve ID defining the maximum shear stress at failure as a function of the effective strain rate. Input as a negative number. USRVn Failure constants for user failure subroutine, 𝑛 = 1,2, … ,6 ZD ZT Notch diameter Sheet thickness. ZALP1 Correction factor alpha1 ZALP2 Correction factor alpha2 ZALP3 Correction factor alpha3 ZRRAD Notch root radius (OPT = 3.0 only). ZT2 LCT 2-514 (EOS) Second sheet thickness (OPT = 5.0 only) VARIABLE DESCRIPTION LCC RS OPT under tension as a function of loading direction (in degree range 0 to 90). Table defines these curves as functions of strain rates. See remarks. (OPT = 11.0 only) Load curve or Table ID. Load curve defines resultant failure force under compression as a function of loading direction (in degree range 0 to 90). Table defines these curves as functions of strain rates. See remarks. (OPT = 11.0 only) Rupture strain. Define if and only if damage is active. Failure option: EQ.-9: OPT = 9 failure is evaluated and written to the swforc file, but element failure is suppressed. EQ.-2: same as option –1 but in addition, the peak value of the failure criteria and the time it occurs is stored and is written into the swforc database. This information may be necessary since the instantaneous values written at specified time intervals may miss the peaks. Additional storage is allocated to store this information. EQ.-1: OPT = 0 failure is evaluated and written into the swforc file, but element failure is suppressed EQ.0: resultant based failure EQ.1: stress based failure computed from resultants (Toyota) EQ.2: user subroutine uweldfail to determine failure EQ.3: notch stress based failure. (beam and hex assembly welds only). EQ.4: stress intensity factor at failure. (beam and hex assembly welds only). EQ.5: structural stress at failure (beam and hex assembly welds only). EQ.6: stress based failure computed from resultants (Toyota). In this option a shell strain rate dependent failure model is used (beam and hex assembly welds only). The static failure stresses are defined by part ID using the keyword *DEFINE_SPOTWELD_RUPTURE_STRESS. EQ.7: stress based failure for solid elements (Toyota) with peak stresses computed from resultants, and strength values input for pairs of parts, see *DEFINE_SPOTWELD_- VARIABLE DESCRIPTION FAILURE_RESULTANTS. Strain rate effects are option- al. EQ.8: not used. EQ.9: stress based failure from resultants (Toyota). In this option a shell strain rate dependent failure model is used (beam welds only). The static failure stresses are defined by part ID using the keyword *DEFINE_SPOTWELD_- RUPTURE_PARAMETER. EQ.10: stress based failure with rate effects. Failure data is defined by material using the keyword *DEFINE_- SPOWELD_FAILURE. EQ.11: resultant based failure (beams only). In this option load curves or tables LCT (tension) and LCC (compression) can be defined as resultant failure force vs. loading di- rection (curve) or resultant failure force vs. loading di- rection vs. strain rate (table). EQ.12: user subroutine uweldfail12 with 22 material constants to determine damage and failure. EQ.22: user subroutine uweldfail22 with 22 material constants to determine failure. FVAL Failure parameter. If OPT: EQ.-2: Not used. EQ.-1: Not used. EQ.0: Function ID (*DEFINE_FUNCTION) define alternative Weld Failure. If this is set, the values given for NRR, NRS, NRT, MRR, MSS and MTT in Card 2 are ignored. to EQ.1: Not used. EQ.2: Not used. EQ.3: Notch stress value at failure (KF). EQ.4: Stress intensity factor value at failure (KeqF). EQ.5: Structural stress value at failure (sF). EQ.6: Number of cycles that failure condition must be met to trigger beam deletion. EQ.7: Not used. n5 n8 n4 n6 n7 n3 n1 n2 Figure M100-1. A solid element used as spot weld is shown. When resultant based failure is used orientation is very important. Nodes n1-n4 attach to the lower shell mid-surface and nodes n5-n8 attach to the upper shell mid-surface. The resultant forces and moments are computed based on the assumption that the brick element is properly oriented. VARIABLE DESCRIPTION TRUE_T EQ.9: Number of cycles that failure condition must be met to trigger beam deletion. EQ.10: ID of data defined by *DEFINE_SPOTWELD_FAILURE. True weld thickness. This optional value is available for solid element failure, and is used to reduce the moment contribution to the failure calculation from artificially thick weld elements under shear loading so shear failure can be modeled more accurately. See comments under the remarks for *MAT_SPOTWELD_DAIM- LER CHRYSLER ASFF Weld assembly simultaneous failure flag EQ.0: Damaged elements fail individually. EQ.1: Damaged elements fail when first reaches failure criterion. BETA Damage model decay rate. DMGOPT Damage option flag. If DMGOPT: EQ.0: Plastic strain based damage. EQ.1: Plastic strain based damage with post damage stress limit VARIABLE DESCRIPTION EQ.2: Time based damage with post damage stress limit EQ.10: Like DMGOPT = 0, but failure option will initiate damage EQ.11: Like DMGOPT = 1, but failure option will initiate damage EQ.12: Like DMGOPT = 2, but failure option will initiate damage FMODE Failure surface ratio for damage or failure, for DMGOPT = 10, 11, or 12 EQ.0: Damage initiates GT.0: Damage or failure FFCAP Failure function limit for OPT = 0 or -1, and DMGOPT = 10, 11, or 12 EQ.0: Damage initiates GT.0: Damage or failure USRVn Failure constants for OPT = 12 or 22 user defined failure, 𝑛 = 7, 8, … , 22 Weld Failure Spot weld material is modeled with isotropic hardening plasticity coupled to failure models. EFAIL specifies a failure strain which fails each integration point in the spot weld independently. The OPT parameter is used to specify a failure criterion that fails the entire weld element when the criterion is met. Alternatively, EFAIL and OPT option may be used to initiate damage when the DAMAGE-FAILURE option is active using RS, BETA, and DMGOPT as described below. Beam spot weld elements can use any OPT value except 7. Brick spot weld elements can use any OPT value except 3, 4, 5, 6, 9, and -9. Hex assembly spot welds can use any OPT value except 9 and -9. OPT = -1 or 0 OPT = 0 and OPT = -1 invoke a resultant-based failure criterion that fails the weld if the resultants are outside of the failure surface defined by: [ max(𝑁𝑟𝑟, 0) 𝑁𝑟𝑟𝐹 ] ] + [ 𝑁𝑟𝑠 𝑁𝑟𝑠𝐹 + [ 𝑁𝑟𝑡 𝑁𝑟𝑡𝐹 ] ] + [ 𝑀𝑟𝑟 𝑀𝑟𝑟𝐹 + [ 𝑀𝑠𝑠 𝑀𝑠𝑠𝐹 ] ] + [ 𝑀𝑡𝑡 𝑀𝑡𝑡𝐹 − 1 = 0 where the numerators in the equation are the resultants calculated in the local coordinates of the cross section, and the denominators are the values specified in the input. If OPT = -1, the failure surface equation is evaluated, but element failure is suppressed. This allows easy identification of vulnerable spot welds when post- processing. Failure is likely to occur if FC > 1.0. Alternatively a *DEFINE_FUNCTION could be used to define the Weld Failure for OPT = 0. Then set FVAL = function ID. Such a function could look like this: *DEFINE_FUNCTION 100 func(nrr,nrs,nrt,mrr,mss,mtt)= (nrr/5.0)*(nrr/5.0) The six arguments for this function (nrr, …, mtt) are the force and moment resultants during the computation. OPT = 1: OPT = 1 invokes a stress based failure model, which was developed by Toyota Motor Corporation and is based on the peak axial and transverse shear stresses. The weld fails if the stresses are outside of the failure surface defined by ( 𝜎𝑟𝑟 𝐹 ) 𝜎𝑟𝑟 + ( 𝜏𝐹) − 1 = 0 If strain rates are considered then the failure criteria becomes: [ 𝜎𝑟𝑟 ] 𝐹 (𝜀̇eff) 𝜎𝑟𝑟 + [ ] 𝜏𝐹(𝜀̇eff) − 1 = 0 where 𝜎𝑟𝑟 stresses are calculated from the resultants using simple beam theory. 𝐹 (𝜀̇eff) and 𝜏𝐹(𝜀̇eff) are defined by load curves LCAX and LCTAU. The peak 𝜎𝑟𝑟 = 𝑁𝑟𝑟 + 2 + 𝑀𝑡𝑡 √𝑀𝑠𝑠 2 + 𝑁𝑟𝑡 √𝑁𝑟𝑠 where the area and section modulus are given by: 𝑀𝑟𝑟 2𝑍 𝜏 = + 𝐴 = 𝜋 𝑍 = 𝜋 𝑑2 𝑑3 32 and d is the equivalent diameter of the beam element or solid element used as a spot weld. *MAT_SPOTWELD OPT = 2 invokes a user-written subroutine uweldfail, documented in Appendix Q. OPT = 12 or 22 OPT = 12 and OPT = 22 invoke similar user-written subroutines, uweldfail12, or, uweldfail22 respectively. Both allow up to 22 failure parameters to be used rather than the 6 allowed with OPT = 2. OPT = 12 also allows user control of weld damage. OPT = 3 OPT = 3 invokes a failure based on notch stress, see Zhang [1999]. Failure occurs when the failure criterion: is satisfied. The notch stress is given by the equation: 𝜎𝑘 − 𝜎𝑘𝐹 ≥ 0 𝜎𝑘 = 𝛼1 ⎜⎛1 + 4𝐹 𝜋𝑑𝑡 ⎝ √3 + √19 8√𝜋 √ ⎟⎞ + 𝛼2 𝜌⎠ 6𝑀 𝜋𝑑𝑡2 ⎜⎛1 + ⎝ √3𝜋 √ ⎟⎞ + 𝛼3 𝜌⎠ 4𝐹𝑟𝑟 𝜋𝑑2 ⎜⎛1 + ⎝ 3√2𝜋 √ ⎟⎞ 𝜌⎠ Here, 𝐹 = √𝐹𝑟𝑠 2 2 + 𝐹𝑟𝑡 𝑀 = √𝑀𝑠𝑠 2 2 + 𝑀𝑡𝑡 and 𝛼𝑖 𝑖 = 1,2,3 are input corrections factors with default values of unity. If spot welds are between sheets of unequal thickness, the minimum thickness of the spot welded sheets may be introduced as a crude approximation. OPT = 4 OPT = 4 invokes failure based on structural stress intensity, see Zhang [1999]. Failure occurs when the failure criterion: is satisfied where and 𝐾eq − 𝐾eqF ≥ 0 𝐾eq = √𝐾𝐼 2 2 + 𝐾𝐼𝐼 𝐾𝐼 = 𝛼1 √3𝐹 2𝜋𝑑√𝑡 + 𝛼2 2√3𝑀 𝜋𝑑𝑡√𝑡 + 𝛼3 5√2𝐹𝑟𝑟 3𝜋𝑑√𝑡 𝐾𝐼𝐼 = 𝛼1 2𝐹 𝜋𝑑√𝑡 Here, F and M are as defined above for the notch stress formulas and again, 𝛼𝑖 𝑖 = 1,2,3 are input corrections factors with default values of unity. If spot welds are between sheets of unequal thickness, the minimum thickness of the spot welded sheets may be used as a crude approximation. The maximum structural stress at the spot weld was utilized successfully for predicting the fatigue failure of spot welds, see Rupp, et. al. [1994] and Sheppard [1993]. The corresponding results according to Rupp, et. al. are listed below where it is assumed that they may be suitable for crash conditions. OPT = 5 OPT = 5 invokes failure by max(𝜎𝑣1, 𝜎𝑣2, 𝜎𝑣3) − 𝜎𝑠𝐹 = 0 where 𝜎𝑠𝐹 is the critical value of structural stress at failure. It is noted that the forces and moments in the equations below are referred to the beam nodes 1, 2, and to the midpoint, respectively. The three stress values, 𝜎𝑣1, 𝜎𝑣2, 𝜎𝑣3, are defined by: 𝜎𝑣1(𝜁 ) = 𝐹𝑟𝑠1 𝜋𝑑𝑡1 cos𝜁 + 𝐹𝑟𝑡1 𝜋𝑑𝑡1 sin𝜁 − 1.046𝛽1𝐹𝑟𝑟1 𝑡1√𝑡1 − 1.123𝑀𝑠𝑠1 𝑑𝑡1√𝑡1 sin𝜁 + 1.123𝑀𝑡𝑡1 𝑑𝑡1√𝑡1 cos𝜁 with 𝛽1 = { 0 𝐹𝑟𝑟1 ≤ 0 1 𝐹𝑟𝑟1 > 0 𝜎𝑣2(𝜁 ) = 𝐹𝑟𝑠2 𝜋𝑑𝑡2 cos𝜁 + 𝐹𝑟𝑡2 𝜋𝑑𝑡2 sin𝜁 − 1.046𝛽1𝐹𝑟𝑟2 𝑡2√𝑡2 + 1.123𝑀𝑠𝑠2 𝑑𝑡2√𝑡2 sin𝜁 − 1.123𝑀𝑡𝑡2 𝑑𝑡2√𝑡2 cos𝜁 with where 𝛽2 = { 0 𝐹𝑟𝑟2 ≤ 0 1 𝐹𝑟𝑟2 > 0 𝜎𝑣3(𝜁 ) = 0.5𝜎(𝜁 ) + 0.5𝜎(𝜁 )cos(2𝛼) + 0.5𝜏(𝜁 )sin(2𝛼) 𝜎(𝜁 ) = 𝜏(𝜁 ) = 𝛼 = 32𝑀𝑡𝑡 𝜋𝑑3 cos𝜁 32𝑀𝑠𝑠 𝜋𝑑3 sin𝜁 − 16𝐹𝑟𝑡 3𝜋𝑑2 cos2𝜁 4𝛽3𝐹𝑟𝑟 𝜋𝑑2 + 16𝐹𝑟𝑠 3𝜋𝑑2 sin2𝜁 + tan−1 2𝜏(𝜁 ) 𝜎(𝜁 ) 𝛽3 = { 0 𝐹𝑟𝑟 ≤ 0 1 𝐹𝑟𝑟 > 0 The stresses are calculated for all directions, 0° ≤ 𝜁 ≤ 90°, in order to find the maximum. OPT = 10 OPT = 10 invokes the failure criterion developed by Lee and Balur (2011). It is available for welds modeled by beam elements, solid elements, or solid assemblies. A detailed discussion of the criterion is given in the user’s manual section for *DEFINE_- SPOTWELD_FAILURE. OPT = 11 OPT = 11 invokes a resultant force based failure criterion for beams. With correspond- ing load curves or tables LCT and LCC, resultant force at failure 𝐹𝑓𝑎𝑖𝑙 can be defined as function of loading direction 𝛾 (curve ) or loading direction 𝛾 and effective strain rate 𝜀̇ (table): with the following definitions for loading direction (in degree) and effective strain rate: 𝐹fail = 𝑓 (𝛾) or 𝐹fail = 𝑓 (𝛾, 𝜀̇) 𝛾 = tan−1 (∣ 𝐹shear 𝐹axial ∣) , 𝜀̇ = [ (𝜀̇axial 2 + 𝜀shear 2 ̇ )] 1/2 It depends on the sign of the axial beam force, if LCT or LCC are used for failure condition: 𝐹axial > 0: [𝐹axial 2 + 𝐹shear 𝐹axial < 0: [𝐹axial 2 + 𝐹shear 1/2 ] 1/2 ] > Ffail,LCT → failure > Ffail,LCC → failure For all OPT failure criteria, if a zero is input for a failure parameter on card 2, the corresponding term will be omitted from the equation. For example, if for OPT = 0, only 𝑁𝑟𝑟𝐹 is nonzero, the failure surface is reduced to |𝑁𝑟𝑟| = 𝑁𝑟𝑟𝐹. Similarly, if the failure strain EFAIL is set to zero, the failure strain model is not used. Both EFAIL and OPT failure may be active at the same time. NF specifies the number of terms used to filter the stresses or resultants used in the OPT failure criterion. NF cannot exceed 30. The default value is set to zero which is generally recommended unless oscillatory resultant forces are observed in the time history databases. Although welds should not oscillate significantly, this option was added for consistency with the other spot weld options. NF affects the storage since it is necessary to store the resultant forces as history variables. The NF parameter is available only for beam element welds. The inertias of the spot welds are scaled during the first time step so that their stable time step size is Δ𝑡. A strong compressive load on the spot weld at a later time may reduce the length of the spot weld so that stable time step size drops below Δ𝑡. If the value of Δ𝑡 is zero, mass scaling is not performed, and the spot welds will probably limit the time step size. Under most circumstances, the inertias of the spot welds are small enough that scaling them will have a negligible effect on the structural response and the use of this option is encouraged. Spot weld force history data is written into the swforc ASCII file. In this database the resultant moments are not available, but they are in the binary time history database and in the ASCII elout file. Damage When the DAMAGE-FAILURE option is invoked, the constitutive properties for the damaged material are obtained from the undamaged material properties. The amount of damage evolved is represented by the constant, 𝜔, which varies from zero if no damage has occurred to unity for complete rupture. For uniaxial loading, the nominal stress in the damaged material is given by 𝜎nominal = where P is the applied load and A is the surface area. The true stress is given by: where 𝐴loss is the void area. The damage variable can then be defined: 𝜎true = 𝐴 − 𝐴loss where, 𝜔 = 𝐴loss 0 ≤ 𝜔 ≤ 1 In this model, damage is initiated when the effective plastic strain in the weld exceeds the failure strain, EFAIL. If DMGOPT = 10, 11, or 12, damage will initiate when the effective plastic strain exceeds EFAIL, or when the failure criterion is met, which ever occurs first. The failure criterion is specified by OPT parameter. After damage initiates, the damage variable is evaluated by one of two ways. For DMGOPT = 0, 1, 10, or 11, the damage variable is a function of effective plastic strain in the weld: 𝜀failure ≤ 𝜀eff 𝑝 ≤ 𝜀rupture ⇒ 𝜔 = 𝑝 − 𝜀failure 𝜀eff − 𝜀failure 𝜀rupture where 𝜀failure a function of time: = EFAIL and 𝜀rupture = RS. For DMGOPT = 2 or 12, the damage variable is 𝑡failure ≤ 𝑡 ≤ 𝑡rupture ⇒ 𝜔 = 𝑡 − 𝑡failure 𝑡rupture where 𝑡failure is the time at which damage initiates, and 𝑡rupture = RS. For this criteria, 𝑝 exceeds EFAIL, or the time when the failure 𝑡failure is set to either the time when 𝜀eff criterion is met. For DMGOPT = 1, the damage behavior is the same as for DMGOPT = 0, but an additional damage variable is calculated to prevent stress growth during softening. Similarly, DMGOPT = 11 behaves like DMGOPT = 10 except for the additional damage variable. This additional function is also used with DMGOPT = 2 and 12. The effect of this additional damage function is noticed only in brick and brick assembly welds in tension loading where it prevents growth of the tensile force in the weld after damage initiates. For DMGOPT = 10, 11, or 12 an optional FMODE parameter determines whether a weld that reaches the failure surface will fail immediately, or initiate damage. The failure surface calculation has shear terms, which may include the torsional moment, and also normal and bending terms. If FMODE is input with a value between 0 and 1, then when the failure surface is reached, the sum of the square of the shear terms is divided by the sum of the square of all terms. If this ratio exceeds FMODE, then the weld will fail immediately. If the ratio is less than or equal to FMODE, then damage will initiate. The FMODE option is available only for brick and brick assembly welds. For resultant based failure (OPT = -1 or 0) and DMGOPT = 10, 11, or 12 an optional FFCAP parameter determines whether a weld that reaches the failure surface will fail immediately. After damage initiation, the failure function can reach values above 1.0. This can now be limited by the FFCAP value (should be larger than 1.0): max(𝑁𝑟𝑟, 0) ] 𝑁𝑟𝑟𝐹 ⎜⎛[ ⎝ + [ 𝑁𝑟𝑠 𝑁𝑟𝑠𝐹 ] ] + [ 𝑁𝑟𝑡 𝑁𝑟𝑡𝐹 + [ 𝑀𝑟𝑟 𝑀𝑟𝑟𝐹 ] + [ 𝑀𝑠𝑠 𝑀𝑠𝑠𝐹 ] + [ 𝑀𝑡𝑡 𝑀𝑡𝑡𝐹 ] ⎟⎞ ⎠ < FFCAP BETA If BETA is specified, the stress is multiplied by an exponential using ω defined in the previous equations, 𝜎𝑑 = 𝜎exp(−𝛽𝜔). For weld elements in an assembly , the failure criterion is evaluated using the assembly cross section. If damage is not active, all elements will be deleted when the failure criterion is met. If damage is active, then damage is calculated independently in each element of the assembly. By default, elements of the assembly are deleted as damage in each element is complete. If ASFF = 1, then failure and deletion of all elements in the assembly will occur simultaneously when damage is complete in any one of the elements. TRUE_T Weld elements and weld assemblies are tied to the mid-plane of shell materials and so typically have a thickness that is half the sum of the thicknesses of the welded shell sections. As a result, a weld under shear loading can be subject to an artificially large moment which will be balanced by normal forces transferred through the tied contact. These normal forces will cause the out-of-plane bending moment used in the failure calculation to be artificially high. Inputting a TRUE_T that is smaller than the modeled thickness, for example, 10%-30% of true thickness will scale down the moment or stress that results from the balancing moment and provide more realistic failure calculations for solid elements and weld assemblies. TRUE_T effects only the failure calculation, not the weld element behavior. If TRUE_T = 0 or data is omitted, the modeled weld element thickness is used. For OPT = 0, the two out-of-plane moments, 𝑀𝑠𝑠 and 𝑀𝑡𝑡 are replaced by modified terms 𝑀̂𝑠𝑠 and 𝑀̂𝑡𝑡, as shown below: [ max(𝑁𝑟𝑟, 0) 𝑁𝑟𝑟𝐹 ] ] + [ 𝑁𝑟𝑠 𝑁𝑟𝑠𝐹 + [ 𝑁𝑟𝑡 𝑁𝑟𝑡𝐹 ] ] + [ 𝑀𝑟𝑟 𝑀𝑟𝑟𝐹 + [ 𝑀̂𝑠𝑠 𝑀𝑠𝑠𝐹 ] ] + [ 𝑀̂𝑡𝑡 𝑀𝑡𝑡𝐹 − 1 = 0 𝑀̂𝑠𝑠 = 𝑀𝑠𝑠 − 𝑁𝑟𝑡(𝑡 − 𝑡true) 𝑀̂𝑡𝑡 = 𝑀𝑡𝑡 − 𝑁𝑟𝑠(𝑡 − 𝑡true) In the above, 𝑡 is the element thickness and . 𝑡true is the TRUE_T parameter. For OPT = 1, the same modification is done to the moments that contribute to the normal stress, as shown below: 𝜎𝑟𝑟 = 𝑁𝑟𝑟 + √𝑀̂𝑠𝑠 2 + 𝑀̂ 𝑡𝑡 Uniaxial option A uniaxial stress option is available for solid and solid weld assemblies. It is invoked by defining the elastic modulus, 𝐸 as a negative number where the absolute value of 𝐸 is the desired value for 𝐸. The uniaxial option causes the two transverse stress terms to be assumed to be zero throughout the calculation. This assumption eliminates parasitic transverse stress that causes slow growth of plastic strain based damage. The motivation for this option can be explained with a weld loaded in tension. Due to Poisson’s effect, an element in tension would be expected to contract in the transverse directions. However, because the weld nodes are constrained to the mid-plane of shell elements, such contraction is only possible to the degree that that shell element contracts. In other words, the uniaxial stress state cannot be represented by the weld. For plastic strain based damage, this effect can be particularly apparent as it causes tensile stress to continue to grow very large as the stress state becomes very nearly triaxial tension. In this stress state, plastic strain grows very slowly so it appears that damage calculation is failing to knock down the stress. By simply assuming that the transverse stresses are zero, the plastic strain grows as expected and damage is much more effective. Material histories The probability of failure in solid or beam spotwelds can be estimated by retrieving the corresponding material histories for output to the d3plot database *DEFINE_MATERIAL_HISTORIES Properties Label Attributes Description Instability Damage - - - - - - - A measure between 0 and 1 related to how close the spotweld element is to fail - Damage in the spotweld element between 0 and 1 These two labels are supported for all options (OPT and DMGOPT, including assemblies and beams), except for user defined failure. The instability measure is the maximum over time; namely, it gives the maximum value for a given element throughout the simulation. If a damage option is invoked then damage will initiate and increment when the instability reaches unity, and elements are not deleted until the damage value reaches unity. If no damage option is invoked then the damage output is always zero and elements will be deleted at the point when the instability measure reaches unity. *MAT_SPOTWELD_DAIMLERCHRYSLER This is Material Type 100. The material model applies only to solid element type l. If hourglass type 4 is specified then hourglass type 4 will be used, otherwise, hourglass type 6 will be automatically assigned. Hourglass type 6 is preferred. constraint Spot weld elements may be placed between any two deformable shell surfaces and tied *CONTACT_TIED_SURFACE_TO_SURFACE, which with eliminates the need to have adjacent nodes at spot weld locations. Spot weld failure is modeled using this card and *DEFINE_CONNECTION_PROPERTIES data. Details of the failure model can be found in Seeger, Feucht, Frank, Haufe, and Keding [2005]. contact, NOTE: It is advisable to include all spot welds, which pro- vide the slave nodes, and spot welded materials, which define the master segments, within a single *CONTACT_TIED_SURFACE_TO_SURFACE inter- face. This contact type uses constraint equations. If multiple interfaces are treated independently, sig- nificant problems can occur if such interfaces share common nodes. An added benefit is that memory usage can be substantially less with a single inter- face . Card 1 1 Variable MID Type A8 Card 2 1 Variable EFAIL Type F 2 RO F 2 3 E F 3 4 PR F 4 5 6 5 6 7 DT F 7 8 TFAIL F 8 NF Card 3 Variable 1 RS 2 3 4 5 6 7 8 ASFF TRUE_T CON_ID JTOL Type F I F F F VARIABLE DESCRIPTION MID RO E PR DT TFAIL EFAIL NF Material identification. A unique number or label not exceeding 8 characters must be specified. Mass density. Young’s modulus. Poisson’s ratio. Time step size for mass scaling, Δ𝑡. Failure time if nonzero. If zero this option is ignored. Effective plastic strain in weld material at failure. See remark below. Number of failure function evaluations stored for filtering by time averaging. The default value is set to zero which is generally recommended unless oscillatory resultant forces are observed in the time history databases. Even though these welds should not oscillate significantly, this option was added for consistency with the other spot weld options. NF affects the storage since it is necessary to store the failure terms. When NF is nonzero, the resultants in the output databases are filtered. NF cannot exceed 30. RS ASFF Rupture strain. See Remarks below. Weld assembly simultaneous failure flag EQ.0: Damaged elements fail individually. EQ.1: Damaged elements fail when first reaches failure criterion. TRUE_T True weld thickness for single hexahedron solid weld elements. See comments below. DESCRIPTION Connection ID of *DEFINE_CONNECTION card. A negative CON_ID deactivates failure, see comments below. Tolerance value for relative volume change (default: JTOL = 0.01). Solid element spotwelds with a Jacobian less than JTOL will be eroded. VARIABLE CON_ID JTOL Remarks: This weld material is modeled with isotropic hardening plasticity. The yield stress and constant hardening modulus are assumed to be those of the welded shell elements as defined in a *DEFINE_CONNECTION_PROPERTIES table. A failure function and damage type is also defined by *DEFINE_CONNECTION_PROPERTIES data. The interpretation of EFAIL and RS is determined by the choice of damage type. This is discussed in remark 4 on *DEFINE_CONNECTION_PROPERTIES. Solid weld elements are tied to the mid-plane of shell materials and so typically have a thickness that is half the sum of the thicknesses of the welded shell sections. As a result, a weld under shear loading can be subject to an artificially large moment which will be balanced by normal forces transferred through the tied contact. These normal forces will cause the normal term in the failure calculation to be artificially high. Inputting a TRUE_T that is smaller than the modeled thickness, for example, 10%-30% of true thickness will scale down the normal force that results from the balancing moment and provide more realistic failure calculations. TRUE_T effects only the failure calculation, not the weld element behavior. If TRUE_T = 0 or data is omitted, the modeled weld element thickness is used. For weld elements in an assembly , the failure criterion is evaluated using the assembly cross section. If damage is not active, all elements will be deleted when the failure criterion is met. If damage is active, then damage is calculated independently in each element of the assembly. By default, elements of the assembly are deleted as damage in each element is complete. If ASFF = 1, then failure and deletion of all elements in the assembly will occur simultaneously when damage is complete in any one of the elements. Solid element force resultants for MAT_SPOTWELD are written to the spot weld force file, swforc, and the file for element stresses and resultants for designated elements, ELOUT. Also, spot weld failure data is written to the file, dcfail. An option to deactivate weld failure is switched on by setting CON_ID to a negative value where the absolute value of CON_ID becomes the connection ID. When weld failure is deactivated, the failure function is evaluated and output to swforc and dcfail but the weld retains its full strength. *MAT_101 is Material Type 101. This The GEPLASTIC_SRATE_2000a material model characterizes General Electric's commercially available engineering thermoplastics subjected to high strain rate events. This material model features the variation of yield stress as a function of strain rate, cavitation effects of rubber modified materials and automatic element deletion of either ductile or brittle materials. Card 1 1 Variable MID Type A8 Card 2 1 2 RO F 2 3 E F 3 4 5 6 7 8 PR RATESF EDOT0 ALPHA F 4 F 5 F 6 F 7 8 Variable LCSS LCFEPS LCFSIG LCE Type F F F F VARIABLE DESCRIPTION MID RO E PR Material identification. A unique number or label not exceeding 8 characters must be specified. Mass density. Young's Modulus. Poisson's ratio. RATESF Constant in plastic strain rate equation. EDOT0 Reference strain rate ALPHA Pressure sensitivity factor LCSS Load curve ID or Table ID that defines the post yield material behavior. The values of this stress-strain curve are the difference of the yield stress and strain respectively. This means the first values for both stress and strain should be zero. All subsequent values will define softening or hardening. Load curve ID that defines the plastic failure strain as a function of strain rate. Load curve ID that defines the Maximum principal failure stress as a function of strain rate. Load curve ID that defines the Unloading moduli as a function of plastic strain. *MAT_101 VARIABLE LCFEPS LCFSIG LCE Remarks: The constitutive model for this approach is: 𝜀̇𝑝 = 𝜀̇0exp{𝐴[𝜎 − 𝑆(𝜀𝑝)]} × exp(−𝑝𝛼𝐴) where 𝜀̇0 and A are rate dependent yield stress parameters, 𝑆(𝜀𝑝) internal resistance (strain hardening) and 𝛼 is a pressure dependence parameter. In this material the yield stress may vary throughout the finite element model as a function of strain rate and hydrostatic stress. Post yield stress behavior is captured in material softening and hardening values. Finally, ductile or brittle failure measured by plastic strain or maximum principal stress respectively is accounted for by automatic element deletion. Although this may be applied to a variety of engineering thermoplastics, GE Plastics have constants available for use in a wide range of commercially available grades of their engineering thermoplastics. *MAT_INV_HYPERBOLIC_SIN_{OPTION} This is Material Type 102. It allows the modeling of temperature and rate dependent plasticity, Sheppard and Wright [1979]. Available options include: <BLANK> THERMAL such that the keyword card can appear as: *MAT_INV_HYPERBOLIC_SIN or *MAT_102 *MAT_INV_HYPERBOLIC_SIN_THERMAL or *MAT_102_T Card 1 for <BLANK> option: Card 1 1 Variable MID 2 RO Type A8 F Card 2 for <BLANK> option: Card 2 1 Variable ALPHA Type F 2 N F 3 E F 3 A F Card 1 for THERMAL option: Card 1 1 2 3 Variable MID RO ALPHA Type A8 F F 4 PR F 4 Q F 4 N F 5 T F 5 G F 5 A F 8 6 HC F 7 VP F 6 7 8 EPS0 LCQ F I 6 Q F 7 G F 8 EPSO *MAT_INV_HYPERBOLIC_SIN Card 2 1 2 3 4 5 6 7 8 Variable LCE LCPR LCCTE Type F F F VARIABLE MID DESCRIPTION Material identification. A unique number or label not exceeding 8 characters must be specified. RO E PR T HC VP Mass density. Young’s Modulus. Poisson’s ratio Initial Temperature. Heat generation coefficient. Formulation for rate effects: EQ.0.0: Scale yield stress (default) EQ.1.0: Viscoplastic formulation. ALPHA α, see Remarks. Not to be confused with coefficient of thermal expansion. N A Q G EPS0 LCQ See Remarks. See Remarks. See Remarks. See Remarks. Minimum strain rate considered in calculating Z. ID of curve specifying parameter Q. GT.0: Q as function of plastic strain. LT.0: Q as function of temperature. VARIABLE DESCRIPTION ID of curve defining Young’s Modulus vs. temperature. ID of curve defining Poisson’s ratio vs. temperature. ID of curve defining coefficient of thermal expansion vs. temperature. LCE LCPR LCCTE Remarks: Resistance to deformation is both temperature and strain rate dependent. The flow stress equation is: 𝜎 = sinh−1 ⎡ ⎢ ⎣ ( ) ⎤ ⎥ ⎦ where 𝑍, the Zener-Holloman temperature compensated strain rate, is: 𝑍 = max(𝜀̇,EPS0) × exp ( GT ) The units of the material constitutive constants are as follows: 𝐴 (1/sec), 𝑁 (dimensionless), 𝛼 (1/MPa), the activation energy for flow, 𝑄(J/mol), and the universal gas constant, 𝐺 (J/mol K). The value of 𝐺 will only vary with the unit system chosen. Typically it will be either 8.3144 J/mol ∞ K, or 40.8825 lb in/mol ∞ R. The final equation necessary to complete our description of high strain rate deformation is one that allows us to compute the temperature change during the deformation. In the absence of a couples thermo-mechanical finite element code we assume adiabatic temperature change and follow the empirical assumption that 90-95% of the plastic work is dissipated as heat. Thus the heat generation coefficient is where 𝜌 is the density of the material and 𝐶𝑣 is the specific heat. HC ≈ 0.9 𝜌𝐶𝑣 *MAT_ANISOTROPIC_VISCOPLASTIC This is Material Type 103. This anisotropic-viscoplastic material model applies to shell and brick elements. The material constants may be fit directly or, if desired, stress versus strain data may be input and a least squares fit will be performed by LS-DYNA to determine the constants. Kinematic or isotopic or a combination of kinematic and isotropic hardening may be used. A detailed description of this model can be found in the following references: Berstad, Langseth, and Hopperstad [1994]; Hopperstad and Remseth [1995]; and Berstad [1996]. Failure is based on effective plastic strain or by a user defined subroutine. Card 1 1 Variable MID Type A8 Card 2 1 2 RO F 2 3 E F 3 4 PR F 4 5 6 7 8 SIGY FLAG LCSS ALPHA F 5 F 6 F 7 F 8 Variable QR1 CR1 QR2 CR2 QX1 CX1 QX2 CX2 Type F Card 3 Variable 1 VK Type F Card 4 1 F 2 F 3 F 4 F 5 VM R00 or F R45 or G R90 or H F 2 F 3 F 4 F 5 F 6 L F 6 F 7 M F 7 F 8 N F 8 Variable AOPT FAIL NUMINT MACF Type F F F Variable 1 XP Type F Card 6 Variable 1 V1 Type F 2 YP F 2 V2 F 3 ZP F 3 V3 F 4 A1 F 4 D1 F 5 A2 F 5 D2 F 6 A3 F 6 D3 F VARIABLE DESCRIPTION *MAT_103 7 8 7 8 BETA F MID RO E PR Material identification. A unique number or label not exceeding 8 characters must be specified. Mass density. Young’s modulus Poisson’s ratio SIGY Initial yield stress FLAG Flag *MAT_ANISOTROPIC_VISCOPLASTIC DESCRIPTION EQ.0: Give all material parameters EQ.1: Material parameters parameters 𝑄𝑟1, 𝐶𝑟1, 𝑄𝑟2, and 𝐶𝑟2 for pure isotropic hardening (𝛼 = 1) are determined by a least squares fit to the curve or table specified by the variable LCSS. If 𝛼 is input as less than 1, 𝑄𝑟1 and 𝑄𝑟2 are then modified by multiplying them by the factor 𝛼, while the factors 𝑄𝑥1 and 𝑄𝑥2 are taken as the product of the original parameters 𝑄𝑟1and 𝑄𝑟2, resp., for pure iso- tropic hardening and the factor (1 − 𝛼). 𝐶𝑥1 is set equal to 𝐶𝑟1 and 𝐶𝑥2 is set equal to 𝐶𝑟2. 𝛼 is input as variable ALPHA on Card 1 in columns 71-80. EQ.2: Use load curve directly, i.e., no fitting is required for the parameters 𝑄𝑟1, 𝐶𝑟1, 𝑄𝑟2, and 𝐶𝑟2. A table is not allowed and only isotropic hardening is implemented. EQ.4: Use table definition directly, no fitting is required and the values for 𝑄𝑟1, 𝐶𝑟1, 𝑄𝑟2, 𝐶𝑟2, 𝑉𝑘, and 𝑉𝑚 are ignored. Only isotropic hardening is implemented, and this op- tion is only available for solids. LCSS Load curve ID or Table ID. Case 1: LCSS is a Load Curve ID. The load curve ID defines effective stress versus effective plastic strain. Card 2 is ignored with this option. For this load curve case viscoplasticity is modeled when the coefficients 𝑉𝑘 and 𝑉𝑚 are provided. Case 2: LCSS is a Table ID. Table consists of stress versuses effective plastic strain curves indexed by strain rate. See Figure M24-1. FLAG.EQ.1: Table is used to calculate the coefficients 𝑉𝑘 and 𝑉𝑚. FLAG.EQ.4: Table is interpolated and used directly. This option is available only for solid elements. ALPHA 𝛼 distribution of hardening used in the curve-fitting. 𝛼 = 0 pure kinematic hardening and 𝛼 = 1 provides pure isotropic hardening QR1 CR1 Isotropic hardening parameter 𝑄𝑟1 Isotropic hardening parameter 𝐶𝑟1 VARIABLE DESCRIPTION QR2 CR2 QX1 CX1 QX2 CX2 VK VM R00 R45 R90 F G H L M N Isotropic hardening parameter 𝑄𝑟2 Isotropic hardening parameter 𝐶𝑟2 Kinematic hardening parameter 𝑄𝜒1 Kinematic hardening parameter 𝐶𝜒1 Kinematic hardening parameter 𝑄𝜒2 Kinematic hardening parameter 𝐶𝜒2 Viscous material parameter 𝑉𝑘 Viscous material parameter 𝑉𝑚 𝑅00 for shell (Default = 1.0) 𝑅45 for shell (Default = 1.0) 𝑅90 for shell (Default = 1.0) 𝐹 for brick (Default = 1/2) 𝐺 for brick (Default = 1/2) 𝐻 for brick (Default = 1/2) 𝐿 for brick (Default = 3/2) 𝑀 for brick (Default = 3/2) 𝑁 for brick (Default = 3/2) AOPT *MAT_ANISOTROPIC_VISCOPLASTIC DESCRIPTION Material axes option : EQ.0.0: locally orthotropic with material axes determined by element nodes 1, 2, and 4, as with *DEFINE_COORDI- NATE_NODES, and then, for shells only, rotated about the shell element normal by an angle BETA. EQ.1.0: locally orthotropic with material axes determined by a point in space and the global location of the element center; this is the a-direction. This option is for solid elements only. EQ.2.0: globally orthotropic with material axes determined by vectors defined below, as with *DEFINE_COORDI- NATE_VECTOR. EQ.3.0: locally orthotropic material axes determined by rotating the material axes about the element normal by an angle, BETA, from a line in the plane of the element defined by the cross product of the vector v with the element normal. EQ.4.0: locally orthotropic in cylindrical coordinate system with the material axes determined by a vector v, and an originating point, P, which define the centerline ax- is. This option is for solid elements only. LT.0.0: the absolute value of AOPT is a coordinate system ID number (CID on *DEFINE_COORDINATE_NODES, *DEFINE_COORDINATE_SYSTEM or *DEFINE_CO- ORDINATE_VECTOR). Available in R3 version of 971 and later. FAIL Failure flag. LT.0.0: User defined failure subroutine is called to determine failure. This is subroutine named, MATUSR_103, in dyn21.f. EQ.0.0: Failure is not considered. This option is recommended if failure is not of interest since many calculations will be saved. GT.0.0: Plastic strain to failure. When the plastic strain reaches this value, the element is deleted from the calculation. VARIABLE NUMINT DESCRIPTION Number of integration points which must fail before element deletion. If zero, all points must fail. This option applies to shell elements only. For the case of one point shells, NUMINT should be set to a value that is less than the number of through thickness integration points. Nonphysical stretching can sometimes appear in the results if all integration points have failed except for one point away from the midsurface. This is due to the fact that unconstrained nodal rotations will prevent strains from developing at the remaining integration point. In fully integrated shells, similar problems can occur. MACF Material axes change flag for brick elements: EQ.1: No change, default, EQ.2: switch material axes 𝑎 and 𝑏, EQ.3: switch material axes 𝑎 and 𝑐, EQ.4: switch material axes 𝑏 and 𝑐. XP, YP, ZP 𝑥𝑝, 𝑦𝑝, 𝑧𝑝, define coordinates of point 𝐩 for AOPT = 1 and 4. A1, A2, A3 𝑎1, 𝑎2, 𝑎3, define components of vector 𝐚 for AOPT = 2. V1, V2, V3 𝑣1, 𝑣2, 𝑣3 define components of vector 𝐯 for AOPT = 3 and 4. D1, D2, D3 𝑑1, 𝑑2, 𝑑3, define components of vector 𝐝 for AOPT = 2. BETA Material angle in degrees for AOPT = 0 (shells only) and AOPT = 3. BETA may be overridden on the element card, see *ELEMENT_SHELL_BETA and *ELEMENT_SOLID_ORTHO. Remarks: The uniaxial stress-strain curve is given on the following form 𝜎(𝜀eff 𝑝 , 𝜀̇eff 𝑝 ) = 𝜎0 + 𝑄𝑟1[(1 − exp(−𝐶𝑟1𝜀eff + 𝑄𝜒1[(1 − exp(−𝐶𝜒1𝜀eff 𝑝 ))] + 𝑄𝑟2[1 − exp(−𝐶𝑟2𝜀eff 𝑝 ))] + 𝑄𝜒2[(1 − exp(−𝐶𝜒2𝜀eff 𝑝 )] 𝑝 ))] + 𝑉𝑘𝜀̇eff 𝑝 𝑉𝑚 For bricks the following yield criteria is used 𝐹(𝜎22 − 𝜎33)2 + 𝐺(𝜎33 − 𝜎11)2 + 𝐻(𝜎11 − 𝜎22)2 + 2𝐿𝜎23 𝑝 )] = [𝜎(𝜀eff 𝑝 , 𝜀̇eff 2 + 2𝑀𝜎31 2 + 2𝑁𝜎12 𝑝 is the effective plastic strain and 𝜀̇eff 𝑝 is the effective plastic strain rate. For where 𝜀eff shells the anisotropic behavior is given by 𝑅00, 𝑅45 and 𝑅90. The model will work when the three first parameters in card 3 are given values. When 𝑉𝑘 = 0 the material will behave elasto-plastically. Default values are given by: 𝐹 = 𝐺 = 𝐻 = 𝐿 = 𝑀 = 𝑁 = 𝑅00 = 𝑅45 = 𝑅90 = 1 Strain rate of accounted for using the Cowper and Symonds model which, e.g., model 3, scales the yield stress with the factor: ⎜⎛ ⎝ To convert these constants set the viscoelastic constants, 𝑉𝑘 and 𝑉𝑚, to the following values: 1 + 𝑝⁄ 𝜀̇eff ⎟⎞ 𝐶 ⎠ ) 𝑉𝑘 = ( 𝑉𝑚 = If LCSS is nonzero, substitute the initial, quasi-static yield stress for SIGY in the equation for 𝑉𝑘 above. This model properly treats rate effects. The viscoplastic rate formulation is an option in other plasticity models in LS-DYNA, e.g., mat_3 and mat_24, invoked by setting the parameter VP to 1. *MAT_103_P This is Material Type 103_P. This anisotropic-plastic material model is a simplified version of the MAT_ANISOTROPIC_VISCOPLASTIC above. This material model applies only to shell elements. Card 1 1 Variable MID Type A8 Card 2 1 2 RO F 2 3 E F 3 4 PR F 4 Variable QR1 CR1 QR2 CR2 Type F Card 3 1 F 2 F 3 F 4 5 6 7 8 SIGY LCSS F 5 F 6 7 8 5 6 7 8 Variable R00 R45 R90 S11 S22 S33 S12 Type F Card 4 1 Variable AOPT Type F Card 5 Variable 1 XP Type F F 2 2 YP F F 3 3 ZP F F 4 4 A1 F F 5 5 A2 F F 6 6 A3 F F 7 8 7 Card 6 Variable 1 V1 Type F 2 V2 F 3 V3 F 4 D1 F 5 D2 F 6 D3 F 7 8 BETA F VARIABLE DESCRIPTION MID RO E PR SIGY LCSS QR1 CR1 QR2 CR2 R00 R45 R90 S11 S22 S33 Material identification. A unique number or label not exceeding 8 characters must be specified. Mass density. Young’s modulus Poisson’s ratio Initial yield stress Load curve ID. The load curve ID defines effective stress versus effective plastic strain. Card 2 is ignored with this option. Isotropic hardening parameter 𝑄𝑟1 Isotropic hardening parameter 𝐶𝑟1 Isotropic hardening parameter 𝑄𝑟2 Isotropic hardening parameter 𝐶𝑟2 𝑅00 for anisotropic hardening 𝑅45 for anisotropic hardening 𝑅90 for anisotropic hardening Yield stress in local 𝑥-direction. This input is ignored if (𝑅00, 𝑅45, 𝑅90) > 0. Yield stress in local 𝑦-direction. This input is ignored if (𝑅00, 𝑅45, 𝑅90) > 0. Yield stress in local 𝑧-direction. This input is ignored if (𝑅00, 𝑅45, 𝑅90) > 0. VARIABLE DESCRIPTION S12 AOPT Yield stress in local -direction. This input is ignored if (𝑅00, 𝑅45, 𝑅90) > 0. Material axes option : EQ.0.0: locally orthotropic with material axes determined by element nodes 1, 2, and 4, as with *DEFINE_COORDI- NATE_NODES, and then rotated about the shell ele- ment normal by an angle BETA. EQ.2.0: globally orthotropic with material axes determined by vectors defined below, as with *DEFINE_COORDI- NATE_VECTOR. EQ.3.0: locally orthotropic material axes determined by rotating the material axes about the element normal by an angle, BETA, from a line in the plane of the element defined by the cross product of the vector v with the element normal. LT.0.0: the absolute value of AOPT is a coordinate system ID number (CID on *DEFINE_COORDINATE_NODES, *DEFINE_COORDINATE_SYSTEM or *DEFINE_CO- ORDINATE_VECTOR). Available in R3 version of 971 and later. XP, YP, ZP 𝑥𝑝, 𝑦𝑝, 𝑧𝑝 define coordinates of point 𝐩 for AOPT = 1 and 4. A1, A2, A3 𝑎1, 𝑎2, 𝑎3 define components of vector 𝐚 for AOPT = 2. D1, D2, D3 𝑑1, 𝑑2, 𝑑3 define components of vector 𝐝 for AOPT = 2. V1, V2, V3 𝑣1, 𝑣2, 𝑣3 define components of vector 𝐯 for AOPT = 3 and 4. BETA Material angle in degrees for AOPT = 0 and 3, may be overridden on the element card, see *ELEMENT_SHELL_BETA. Remarks: If no load curve is defined for the effective stress versus effective plastic strain, the uniaxial stress-strain curve is given on the following form 𝜎(𝜀eff 𝑝 ) = 𝜎0 + 𝑄𝑟1[1 − exp(−𝐶𝑟1𝜀eff 𝑝 )] + 𝑄𝑟2[1 − exp(−𝐶𝑟2𝜀eff 𝑝 )] 𝑝 is the effective plastic strain. For shells the anisotropic behavior is given by where 𝜀eff 𝑅00, 𝑅45 and 𝑅90, or the yield stress in the different direction. Default values are given by: if the variables R00, R45, R90, S11, S22, S33 and S12 are set to zero. 𝑅00 = 𝑅45 = 𝑅90 = 1 *MAT_104 This is Material Type 104. This is a continuum damage mechanics (CDM) model which includes anisotropy and viscoplasticity. The CDM model applies to shell, thick shell, and brick elements. A more detailed description of this model can be found in the paper by Berstad, Hopperstad, Lademo, and Malo [1999]. This material model can also model anisotropic damage behavior by setting the FLAG to -1 in Card 2. 3 E F 3 Q2 F 3 4 PR F 4 C2 F 4 Card 1 1 Variable MID 2 RO Type A8 F 2 C1 F 2 Card 2 Variable 1 Q1 Type F Card 3 Variable 1 VK Type F Card 4 1 VM R00 or F R45 or G R90 or H F 2 F 3 F 4 Variable AOPT CPH MACF Type F F I 5 6 7 8 SIGY LCSS LCDS F 5 6 7 8 EPSD S or EPSR DC FLAG F 5 F 5 Y0 F F 6 L F 6 F 7 M F 7 F 8 N F 8 ALPHA THETA ETA F F Variable 1 XP Type F Card 6 Variable 1 V1 Type F 2 YP F 2 V2 F 3 ZP F 3 V3 F 4 A1 F 4 D1 F 5 A2 F 5 D2 F 6 A3 F 6 D3 F *MAT_DAMAGE_1 7 8 7 8 BETA F VARIABLE DESCRIPTION MID RO E PR SIGY LCSS Material identification. A unique number or label not exceeding 8 characters must be specified. Mass density Young’s modulus Poisson’s ratio Initial yield stress, 𝜎0 Load curve ID defining effective stress versus effective plastic strain. Isotropic hardening parameters on Card 2 are ignored with this option. LCDS Load curve ID defining nonlinear damage curve. For FLAG = -1. Q1 C1 Q2 C2 EPSD S Isotropic hardening parameter 𝑄1 Isotropic hardening parameter 𝐶1 Isotropic hardening parameter 𝑄2 Isotropic hardening parameter 𝐶2 Damage threshold 𝜀eff,d material softening begins. (Default = 0.0) . Damage effective plastic strain when Damage material constant 𝑆. (Default = 𝜎0 200). For FLAG ≥ 0. VARIABLE DESCRIPTION EPSR DC Effective plastic strain at which material ruptures (logarithmic). For FLAG = -1. Critical damage value 𝐷𝐶. When the damage value 𝐷 reaches this value, the element is deleted from the calculation. (Default = 0.5) For FLAG ≥ 0. FLAG Flag EQ.-1: Anisotropic damage EQ.0: Standard isotropic damage (default) EQ.1: Standard isotropic damage plus strain localization check (only for shell elements) EQ.10: Enhanced isotropic damage EQ.11: Enhanced isotropic damage plus strain localization check (only for shell elements) VK VM R00 R45 R90 F G H L M N Viscous material parameter 𝑉𝑘 Viscous material parameter 𝑉𝑚 𝑅00 for shell (Default = 1.0) 𝑅45 for shell (Default = 1.0) 𝑅90 for shell (Default = 1.0) F for brick (Default = 1/2) G for brick (Default = 1/2) H for brick (Default = 1/2) L for brick (Default = 3/2) M for brick (Default = 3/2) N for brick (Default = 3/2) AOPT Material axes option : EQ.0.0: locally orthotropic with material axes determined by element nodes 1, 2, and 4, as with *DEFINE_COORDI- NATE_NODES, and then, for shells only, rotated about *MAT_DAMAGE_1 DESCRIPTION the shell element normal by an angle BETA. EQ.1.0: locally orthotropic with material axes determined by a point in space and the global location of the element center; this is the a-direction. This option is for solid elements only. EQ.2.0: globally orthotropic with material axes determined by vectors defined below, as with *DEFINE_COORDI- NATE_VECTOR. EQ.3.0: locally orthotropic material axes determined by rotating the material axes about the element normal by an angle, BETA, from a line in the plane of the element defined by the cross product of the vector v with the element normal. EQ.4.0: locally orthotropic in cylindrical coordinate system with the material axes determined by a vector v, and an originating point, P, which define the centerline ax- is. This option is for solid elements only. LT.0.0: the absolute value of AOPT is a coordinate system ID number (CID on *DEFINE_COORDINATE_NODES, *DEFINE_COORDINATE_SYSTEM or *DEFINE_CO- ORDINATE_VECTOR). Available in R3 version of 971 and later. CPH Microdefects closure parameter h (FLAG ≥ 10). for enhanced damage MACF Material axes change flag for brick elements: EQ.1: No change, default, EQ.2: switch material axes a and b, EQ.3: switch material axes a and c, EQ.4: switch material axes b and c. Y0 Initial damage energy release rate Y0 for enhanced damage (FLAG ≥ 10). ALPHA Exponent 𝛼 for enhanced damage (FLAG ≥ 10) THETA Exponent 𝜃 for enhanced damage (FLAG ≥ 10) ETA Exponent 𝜂 for enhanced damage (FLAG ≥ 10) VARIABLE DESCRIPTION XP, YP, ZP 𝑥𝑝, 𝑦𝑝, 𝑧𝑝: define coordinates of point 𝐩 for AOPT = 1 and 4 A1, A2, A3 𝑎1, 𝑎2, 𝑎3: define components of vector 𝐚 for AOPT = 2 D1, D2, D3 𝑑1, 𝑑2, 𝑑3: define components of vector 𝐝 for AOPT = 2 V1, V2, V3 𝑣1, 𝑣2, 𝑣3: define components of vector 𝐯 for AOPT = 3 and 4 BETA Μaterial angle in degrees for AOPT = 0 (shells only) and AOPT = 3. BETA may be overridden on the element card, see *ELEMENT_SHELL_BETA and *ELEMENT_SOLID_ORTHO. Remarks: Standard isotropic damage model (FLAG = 0 or 1). The Continuum Damage Mechanics (CDM) model is based on an approach proposed by Lemaitre [1992]. The effective stress 𝜎̃ , which is the stress calculated over the section that effectively resist the forces, reads 𝜎̃ = 1 − 𝐷 where 𝐷 is the damage variable. The evolution equation for the damage variable is defined as 𝐷̇ = ⎧ 0 { ⎨ { ⎩ 𝜀̇eff for for 𝑝 ≤ 𝜀eff,d 𝜀eff 𝑝 > 𝜀eff,d 𝜀eff and 𝜎1 > 0 where 𝜀eff,d 𝜎1 is the maximum principal stress. The damage energy density release rate is is the damage threshold, 𝑆 is the so-called damage energy release rate and 𝑌 = 𝐞𝐞: 𝐂: 𝐞𝐞 = 2 𝑅𝑣 𝜎𝑣𝑚 2𝐸(1 − 𝐷)2 where 𝐸 is Young’s modulus and 𝜎𝑣𝑚 is the equivalent von Mises stress. The triaxiality function 𝑅𝑣 is defined as 𝑅𝑣 = (1 + 𝜈) + 3(1 − 2𝜈) ( 𝜎𝐻 𝜎𝑣𝑚 ) with Poisson’s ratio 𝜈 and hydrostatic stress 𝜎𝐻. Enhanced isotropic damage model (FLAG = 10 or 11). A more sophisticated damage model including crack closure effects (reduced damage under compression) and more flexibility in stress state dependence and functional expressions is invoked by setting FLAG = 10 or 11. The corresponding evolution equation for the damage variable is defined as 𝐷̇ = ( 2𝜏max 𝜎𝑣𝑚 ) ⟨ 𝑌 − 𝑌0 ⟩ 𝑝 (1 − 𝐷)1−𝜃 𝜀̇eff where 𝜏max is the maximum shear stress, 𝑌0 is the initial damage energy release rate and 𝜂, 𝛼, and 𝜃 are additional material constants. 〈 〉 are the Macauley brackets. The damage energy density release rate is 𝑌 = 1 + 𝜈 2𝐸 (∑(〈𝜎̃𝑖〉2 + ℎ〈−𝜎̃𝑖〉2) ) − 𝑖=1 2𝐸 (〈𝜎̃𝐻〉2 + ℎ〈−𝜎̃𝐻〉2) where 𝜎̃𝑖 are the principal effective stresses and h is the microdefects closure parameter that accounts for different damage behavior in tension and compression. A value of ℎ ≈ 0.2 is typically observed in many experiments as stated in Lemaitre [2000]. A parameter set of ℎ = 1, 𝑌0 = 0, 𝛼 = 1, 𝜃 = 1, and 𝜂 = 0 should give the same results as the standard isotropic damage model (FLAG = 0/1) with 𝜀eff,d = 0 as long as 𝜎1 > 0. Strain localization check (FLAG = 1 or 11). In order to add strain localization computation to the damage models above, parameter FLAG should be set to 1 (standard damage) or 11 (enhanced damage). An acoustic tensor based bifurcation criterion is checked and history variable no. 4 is set to 1.0 if strain localization is indicated. Only available for shell elements. Anisotropic damage model (FLAG = -1). At each thickness integration points, an anisotropic damage law acts on the plane stress tensor in the directions of the principal total shell strains, 𝜀1 and 𝜀2, as follows: 𝜎11 = [1 − 𝐷1(𝜀1)]𝜎110 𝜎22 = [1 − 𝐷2(𝜀2)]𝜎220 𝜎12 = [1 − 𝐷1 + 𝐷2 ] 𝜎120 The transverse plate shear stresses in the principal strain directions are assumed to be damaged as follows: 𝜎13 = (1 − 𝐷1/2)𝜎130 𝜎23 = (1 − 𝐷2/2)𝜎230 In the anisotropic damage formulation, 𝐷1(𝜀1) and 𝐷2(𝜀2) are anisotropic damage functions for the loading directions 1 and 2, respectively. Stresses 𝜎110, 𝜎220,𝜎120, 𝜎130 and 𝜎230 are stresses in the principal shell strain directions as calculated from the undamaged elastic-plastic material behavior. The strains 𝜀1 and 𝜀2 are the magnitude of the principal strains calculated upon reaching the damage thresholds. Damage can only develop for tensile stresses, and the damage functions 𝐷1(𝜀1) and 𝐷2(𝜀2)are identical to zero for negative strains 𝜀1 and 𝜀2. The principal strain directions are fixed within an integration point as soon as either principal strain exceeds the initial threshold strain in tension. A more detailed description of the damage evolution for this material model is given in the description of Material 81. Anisotropic viscoplasticity. The uniaxial stress-strain curve is given in the following form 𝜎(𝑟, 𝜀̇eff 𝑝 ) = 𝜎0 + 𝑄1[1 − exp(−𝐶1𝑟)] + 𝑄2[1 − exp(−𝐶2𝑟)] + 𝑉𝑘𝜀̇eff 𝑝 𝑉𝑚 where r is the damage accumulated plastic strain, which can be calculated by 𝑟 ̇ = 𝜀̇eff For bricks the following yield criterion associated with the Hill criterion is used 𝑝 (1 − 𝐷) 𝐹(𝜎̃22 − 𝜎̃33)2 + 𝐺(𝜎̃33 − 𝜎̃11)2 + 𝐻(𝜎̃11 − 𝜎̃22)2 + 2𝐿𝜎̃23 2 + 2𝑀𝜎̃31 2 + 2𝑁𝜎̃12 2 = 𝜎(𝑟, 𝜀̇eff 𝑝 ) 𝑝 is the effective viscoplastic where 𝑟 is the damage effective viscoplastic strain and 𝜀̇eff strain rate. For shells the anisotropic behavior is given by the R-values: 𝑅00, 𝑅45, and 𝑅90. When 𝑉𝑘 = 0 the material will behave as an elastoplastic material without rate effects. Default values for the anisotropic constants are given by: 𝐹 = 𝐺 = 𝐻 = 𝐿 = 𝑀 = 𝑁 = 𝑅00 = 𝑅45 = 𝑅90 = 1 so that isotropic behavior is obtained. Strain rate is accounted for using the Cowper and Symonds model which scales the yield stress with the factor: 1 + ( 𝑝⁄ ) 𝜀̇ To convert these constants, set the viscoelastic constants, 𝑉𝑘 and 𝑉𝑚, to the following values: 𝑉𝑘 = 𝜎 ( ) 𝑉𝑚 = F 0 8 *MAT_105 *MAT_DAMAGE_2 *MAT_DAMAGE_2 This is Material Type 105. This is an elastic viscoplastic material model combined with continuum damage mechanics (CDM). This material model applies to shell, thick shell, and brick elements. The elastoplastic behavior is described in the description of material model 24. A more detailed description of the CDM model is given in the description of material model 104 above. Card 1 1 Variable MID 2 RO Type A8 F 3 E F 4 PR F 5 6 7 8 SIGY ETAN FAIL TDEL F F F Default none none none none none 0.0 10.E+20 Card 2 Variable Type Default 1 C F 0 Card 3 1 Variable EPSD Type F 2 P F 0 2 S F 3 4 5 6 7 LCSS LCSR F 0 4 F 0 3 DC F 5 6 7 8 Default none none none Card 4 1 2 3 4 5 6 7 8 Variable EPS1 EPS2 EPS3 EPS4 EPS5 EPS6 EPS7 EPS8 Type Default F 0 Card 5 1 F 0 2 F 0 3 F 0 4 F 0 5 F 0 6 F 0 7 F 0 8 Variable ES1 ES2 ES3 ES4 ES5 ES6 ES7 ES8 Type Default F 0 F 0 F 0 F 0 F 0 F 0 F 0 F 0 VARIABLE DESCRIPTION MID RO E PR SIGY ETAN FAIL Material identification. A unique number or label not exceeding 8 characters must be specified. Mass density. Young’s modulus. Poisson’s ratio. Yield stress. Tangent modulus, ignored if (LCSS.GT.0) is defined. Failure flag. EQ.0.0: Failure due to plastic strain is not considered. GT.0.0: Plastic strain to failure. When the plastic strain reaches this value, the element is deleted from the calculation. TDEL Minimum time step size for automatic element deletion. C P Strain rate parameter, C, see formula below. Strain rate parameter, P, see formula below. LCSS LCSR EPSD S DC *MAT_DAMAGE_2 DESCRIPTION Load curve ID or Table ID. Load curve ID defining effective stress versus effective plastic strain. If defined EPS1 - EPS8 and ES1 - ES8 are ignored. The table ID defines for each strain rate value a load curve ID giving the stress versus effective plastic strain for that rate, See Figure M24-1. The stress versus effective plastic strain curve for the lowest value of strain rate is used if the strain rate falls below the minimum value. Likewise, the stress versus effective plastic strain curve for the highest value of strain rate is used if the strain rate exceeds the maximum value. The strain rate parameters: C and P; the curve ID, LCSR; EPS1 - EPS8 and ES1 - ES8 are ignored if a Table ID is defined. Load curve ID defining strain rate scaling effect on yield stress. Damage threshold 𝑟𝑑 Damage effective plastic strain when material softening begin. (Default = 0.0) Damage material constant 𝑆. (Default = 𝜎0 200) Critical damage value 𝐷𝐶. When the damage value 𝐷 reaches this value, the calculation. (Default = 0.5) the element is deleted from EPS1 - EPS8 Effective plastic strain values (optional if SIGY is defined). At least 2 points should be defined. ES1 - ES8 Corresponding yield stress values to EPS1 - EPS8. Remarks: The stress-strain behavior may be treated by a bilinear curve by defining the tangent modulus, ETAN. Alternately, a curve similar to that shown in Figure M10-1 is expected to be defined by (EPS1,ES1) - (EPS8,ES8); however, an effective stress versus effective plastic strain curve ID (LCSS) may be input instead if eight points are insufficient. The cost is roughly the same for either approach. The most general approach is to use the table definition with table ID, LCSR, discussed below. Three options to account for strain rate effects are possible. 1. Strain rate may be accounted for using the Cowper and Symonds model which scales the yield stress with the factor 1 + ( 𝑝⁄ ) 𝜀̇ where 𝜀̇ is the strain rate, 𝜀̇ = √𝜀̇𝑖𝑗𝜀̇𝑖𝑗 2. For complete generality a load curve (LCSR) to scale the yield stress may be input instead. In this curve the scale factor versus strain rate is defined. 3. If different stress versus strain curves can be provided for various strain rates, the option using the reference to a table (LCSS) can be used. Then the table input in *DEFINE_TABLE has to be used, see Figure M24-1 A fully viscoplastic formulation is used in this model. *MAT_ELASTIC_VISCOPLASTIC_THERMAL This is Material Type 106. This is an elastic viscoplastic material with thermal effects. Card 1 1 Variable MID Type A8 Card 2 1 2 RO F 2 3 E F 3 4 PR F 4 5 6 7 8 SIGY ALPHA LCSS FAIL F 5 F 6 F 7 F 8 Variable QR1 CR1 QR2 CR2 QX1 CX1 QX2 CX2 Type F Card 3 Variable Type 1 C F Card 4 1 F 2 P F 2 F 3 F 4 F 5 F 6 F 7 F 8 LCE LCPR LCSIGY LCR LCX LCALPH F 3 F 4 F 5 F 6 F 7 F 8 Variable LCC LCP TREF LCFAIL Type F F F F VARIABLE DESCRIPTION MID RO E PR Material identification. A unique number or label not exceeding 8 characters must be specified. Mass density. Young’s modulus Poisson’s ratio VARIABLE DESCRIPTION SIGY LCSS Initial yield stress Load curve ID or Table ID. The load curve ID defines effective stress versus effective plastic strain. The table ID defines for each temperature value a load curve ID giving the stress versus effective plastic strain for that temperature (DEFINE_TABLE) or it defines for each temperature value a table ID which defines for each strain rate a load curve ID giving the stress versus effective plastic strain (DEFINE_TABLE_3D). The stress versus effective plastic strain curve for the lowest value of temperature or strain rate is used if the temperature or strain rate falls below the minimum value. Likewise, maximum values cannot be exceeded. Card 2 is ignored with this option. FAIL Effective plastic failure strain for erosion. ALPHA Coefficient of thermal expansion. QR1 CR1 QR2 CR2 QX1 CX1 QX2 CX2 C P LCE Isotropic hardening parameter 𝑄𝑟1 Isotropic hardening parameter 𝐶𝑟1 Isotropic hardening parameter 𝑄𝑟2 Isotropic hardening parameter 𝐶𝑟2 Kinematic hardening parameter 𝑄𝜒1 Kinematic hardening parameter 𝐶𝜒1 Kinematic hardening parameter 𝑄𝜒2 Kinematic hardening parameter 𝐶𝜒2 Viscous material parameter 𝐶 Viscous material parameter 𝑃 Load curve defining Young's modulus as a function of temperature. E on card 1 is ignored with this option. LCPR Load curve defining Poisson's ratio as a function of temperature. PR on card 1 is ignored with this option. LCSIGY *MAT_ELASTIC_VISCOPLASTIC_THERMAL DESCRIPTION Load curve defining the initial yield stress as a function of temperature. SIGY on card 1 is ignored with this option. LCR LCX Load curve for scaling the isotropic hardening parameters QR1 and QR2 or the stress given by the load curve LCSS as a function of temperature. Load curve for scaling the kinematic hardening parameters QX1 and QX2 as a function of temperature. LCALPH Load curve ID defining the instantaneous coefficient of thermal expansion as a function of temperature: 𝑑𝜀𝑖𝑗 thermal = 𝛼(𝑇)𝑑𝑇𝛿𝑖𝑗 ALPHA on card 1 is ignored with this option. If LCALPH is defined as the negative of the load curve ID, the curve is assumed to define the coefficient relative to a reference temperature, TREF below, such that the total thermal strain is give by thermal = 𝛼(𝑇)(𝑇 − 𝑇ref)𝛿𝑖𝑗 𝜀𝑖𝑗 LCC LCP TREF Load curve for scaling the viscous material parameter C as a function of temperature. Load curve for scaling the viscous material parameter P as a function of temperature. Reference temperature required if and only if LCALPH is given with a negative curve ID. LCFAIL Load curve defining the plastic failure strain as a function of temperature. FAIL on card 1 is ignored with this option. Remarks: If LCSS is not given any value the uniaxial stress-strain curve has the form 𝑝 )] 𝑝 )] + 𝑄𝜒2[1 − exp(−𝐶𝜒2𝜀eff 𝑝 ) = 𝜎0 + 𝑄𝑟1[1 − exp(−𝐶𝑟1𝜀eff 𝑝 )] + 𝑄𝑟2[1 − exp(−𝐶𝑟2𝜀eff + 𝑄𝜒1[1 − exp(−𝐶𝜒1𝜀eff 𝜎(𝜀eff 𝑝 )] Viscous effects are accounted for using the Cowper and Symonds model, which scales the yield stress with the factor: 1 + 𝑝⁄ . 𝜀̇eff ⎟⎞ 𝐶 ⎠ ⎜⎛ ⎝ *MAT_MODIFIED_JOHNSON_COOK This is Material Type 107. Adiabatic heating is included in the material formulation. Material type 107 is not intended for use in a coupled thermal-mechanical analysis or in a mechanical analysis where temperature is prescribed using *LOAD_THERMAL. Define the following two cards with general material parameters Card 1 1 Variable MID Type A8 Card 2 1 Variable E0DOT Type F 2 RO F 2 Tr F 3 E F 3 Tm F 4 PR F 4 T0 F 5 6 BETA XS1 F 5 F 6 FLAG1 FLAG2 F F 7 CP F 7 8 ALPHA F 8 Card 3 for Modified Johnson-Cook Constitutive Relation. This format is used when FLAG1 = 0. Card 3 Variable Type 1 A F 2 B F 3 N F 4 C F 5 m F 6 7 8 Card 4 for Modified Johnson-Cook Constitutive Relation. This format is used when FLAG1 = 0. Card 4 Variable 1 Q1 Type F 2 C1 F 3 Q2 F 4 C2 F 5 6 7 Card 3 for Modified Zerilli-Armstrong Constitutive Relation. This format is used when FLAG1 = 1. Card 3 1 Variable SIGA Type F 2 B F 3 4 5 6 7 8 BETA0 BETA1 F F Card 4 for Modified Zerilli-Armstrong Constitutive Relation. This format is used when FLAG1 = 1. Card 4 Variable Type 1 A F 2 N F 3 4 5 6 7 8 ALPHA0 ALPHA1 F F Card 5 for Modified Johnson-Cook Fracture Criterion. This format is used when FLAG2 = 0. Card 5 Variable 1 DC Type F 2 PD F 3 D1 F 4 D2 F 5 D3 F 6 D4 F 7 D5 F 8 Card 5 for Cockcroft Latham Fracture Criterion. This format is used when FLAG2 = 1. 3 4 5 6 7 8 Card 5 Variable 1 DC 2 WC Type F Additional Element Erosion Criteria Card. Card 6 Variable 1 TC 2 3 4 5 6 7 8 TAUC Type F F VARIABLE DESCRIPTION MID RO E PR Material identification. A unique number or label not exceeding 8 characters must be specified. Mass density Young’s modulus, E. Poisson’s ratio, 𝑣. BETA Damage coupling parameter; see Eq. (107.3). EQ.0.0: No coupling between ductile damage and the constitutive relation. EQ.1.0: Full coupling between ductile damage and the constitutive relation. Taylor-Quinney coefficient 𝜒, see Eq. (107.20). Gives the portion of plastic work converted into heat (normally taken to be 0.9) Specific heat 𝐶𝑝, see Eq. (107.20) XS1 CP ALPHA Thermal expansion coefficient, 𝛼. EPS0 Tr Tm T0 Quasi-static EQ.(107.12).Set description under *MAT_015. threshold strain rate (𝜀̇0 = 𝑝̇0 = 𝑟 ̇0), see Room temperature, see Eq. (107.13) Melt temperature, see Eq. (107.13) Initial temperature VARIABLE DESCRIPTION FLAG1 Constitutive relation flag; see Eq. (107.11) and (107.14) EQ.0.0: Modified Johnson-Cook constitutive relation, see Eq. (107.11). EQ.1.0: Zerilli-Armstrong (107.14). constitutive relation, see Eq. FLAG2 Fracture criterion flag; see Eq. (107.15) and (107.19). EQ.0.0: Modified Johnson-Cook fracture criterion; see Eq. (107.15). EQ.1.0: Cockcroft-Latham fracture criterion; see Eq. (107.19). K G A B N C M Q1 C1 Q2 C2 Bulk modulus Shear modulus Johnson-Cook yield stress A, see Eq. (107.11). Johnson-Cook hardening parameter B, see Eq. (107.11). Johnson-Cook hardening parameter n, see Eq. (107.11). Johnson-Cook strain rate sensitivity parameter C, see Eq. (107.11). Johnson-Cook thermal softening parameter m, see Eq. (107.11). Voce hardening parameter 𝑄1 (when B = n = 0), see Eq. (107.11). Voce hardening parameter 𝐶1 (when B = n = 0), see Eq. (107.11). Voce hardening parameter 𝑄2 (when B = n = 0), see Eq. (107.11). Voce hardening parameter 𝐶2 (when B = n = 0), see Eq. (107.11). SIGA B BETA0 BETA1 Zerilli-Armstrong parameter 𝛼𝑎, see Eq. (107.14). Zerilli-Armstrong parameter 𝐵, see Eq. (107.14). Zerilli-Armstrong parameter 𝛽0, see Eq. (107.14). Zerilli-Armstrong parameter 𝛽1, see Eq. (107.14). A Zerilli-Armstrong parameter 𝐴, see Eq. (107.14). *MAT_MODIFIED_JOHNSON_COOK DESCRIPTION N Zerilli-Armstrong parameter 𝑛, see Eq. (107.14). ALPHA0 Zerilli-Armstrong parameter 𝛼0, see Eq. (107.14). ALPHA1 Zerilli-Armstrong parameter 𝛼1, see Eq. (107.14). DC Critical damage parameter 𝐷𝑐, see Eq. (107.15) and (107.21). When the damage value 𝐷 reaches this value, the element is eroded from the calculation. PD Damage threshold, see Eq. (107.15). D1-D5 Fracture parameters in the Johnson-Cook fracture criterion, see Eq. (107.16). Critical Cockcroft-Latham parameter 𝑊𝑐, see Eq. (107.19). When the plastic work per volume reaches this value, the element is eroded from the simulation. Critical temperature parameter 𝑇𝑐, see Eq. (107.23). When the temperature 𝑇, reaches this value, the element is eroded from the simulation. Critical shear stress parameter 𝜏𝑐. When the maximum shear stress 𝜏 reaches this value, the element is eroded from the simulation. WC TC TAUC Remarks: An additive decomposition of the rate-of-deformation tensor 𝐝 is assumed, i.e. 𝐝 = 𝐝𝑒 + 𝐝𝑝 + 𝐝𝑡 (107.1) Where 𝐝𝑒 is the elastic part, 𝐝𝑝 is the plastic part and 𝐝𝑡 is the thermal part. The elastic rate-of-deformation 𝐝𝑒 is defined by a linear hypo-elastic relation σ̃∇𝐽 = (𝐾 − 𝐺) tr(𝐝𝑒)𝐈 + 𝟐𝐺𝐝𝑒 (107.2) Where 𝐈 is the unit tensor, 𝐾 is the bulk modulus and 𝐺 is the shear modulus. The effective stress tensor is defined by σ̃ = 1 − 𝛽𝐷 (107.3) Where σ is the Cauchy-stress and 𝐷 is the damage variable, while the Jaumann rate of the effective stress reads σ̃∇𝐽 = σ̃̇ − 𝐖 ⋅ σ̃ − σ̃ ⋅ 𝐖𝑇 (107.4) Where 𝐖 is the spin tensor. The parameter 𝛽 is equal to unity for coupled damage and equal to zero for uncoupled damage. The thermal rate-of-deformation 𝐝𝑇 is defined by 𝐝𝑇 = 𝛼𝑇̇𝐈 Where 𝛼 is the linear thermal expansion coefficient and 𝑇 is the temperature. The plastic rate-of-deformation is defined by the associated flow rule as 𝐝𝑝 = 𝑟 ̇ ∂𝑓 ∂σ = 𝑟 ̇ 1 − 𝛽𝐷 σ̃′ 𝜎̃eq (107.5) (107.6) Where (⋅)′ means the deviatoric part of the tensor, 𝑟 is the damage-equivalent plastic strain, 𝑓 is the dynamic yield function, i.e. 𝐝𝑝 = 𝑟 ̇ ∂𝑓 ∂σ = 𝑟 ̇ 1 − 𝛽𝐷 σ̃′ 𝜎̃eq And 𝜎̃eq is the damage-equivalent stress. σ̃′: σ̃′ − 𝜎𝑌(𝑟, 𝑟 ̇, 𝑇) ≤ 0, 𝑓 = √ 𝑟 ̇ ≥ 0, 𝑟 ̇𝑓 = 0 𝜎̃eq = √ σ̃′: σ̃′ The following plastic work conjugate pairs are identified 𝑊̇ 𝑝 = σ: 𝐝𝑝 = 𝜎̃eq𝑟 ̇ = 𝜎eq𝑝̇ (107.6) (107.7) (107.8) (107.9) Where 𝑊̇ 𝑝 is the specific plastic work rate, and the equivalent stress 𝜎eq and the equivalent plastic strain 𝑝 are defined as 𝜎eq = √ σ̃′: σ̃′ = (1 − 𝛽𝐷)𝜎̃eq 𝑝̇ = √ 𝐝𝑝: 𝐝𝑝 = 𝑟 ̇ (1 − 𝛽𝐷) (107.10) The material strength 𝜎𝑌 is defined by: 1. The modified Johnson-Cook constitutive relation 𝜎𝑌 = {𝐴 + 𝐵𝑟𝑛 + ∑ 𝑄𝑖[1 − exp(−𝐶𝑖𝑟)] 𝑖=1 } (1 + 𝑟 ̇∗)𝐶(1 − 𝑇∗𝑚) (107.11) Where 𝐴, 𝐵, 𝐶, 𝑚, 𝑛, 𝑄1, 𝐶1, 𝑄2, 𝐶2 are material parameters; the normalized dam- age-equivalent plastic strain rate 𝑟 ̇∗ is defined by 𝑟 ̇∗ = 𝑟 ̇ 𝜀̇0 (107.12) In which 𝜀̇0 is a user-defined reference strain rate; and the homologous temper- ature reads 𝑇∗ = 𝑇 − 𝑇𝑟 𝑇𝑚 − 𝑇𝑟 (107.13) In which 𝑇𝑟 is the room temperature and 𝑇𝑚 is the melting temperature. 2. The Zerilli-Armstrong constitutive relation 𝜎𝑌 = {𝜎𝑎 + 𝐵exp[−(𝛽0 − 𝛽1ln𝑟 ̇)𝑇] + 𝐴𝑟𝑛exp[−(𝛼0 − 𝛼1ln𝑟 ̇)𝑇]} (107.14) Where 𝜎𝑎, 𝐵, 𝛽0, 𝛽1, 𝐴, 𝑛, 𝛼0, 𝛼1 are material parameters. Damage evolution is defined by: 1. The extended Johnson-Cook damage evolution rule: 𝐷̇ = 𝐷𝑐 𝑝𝑓 − 𝑝𝑑 ⎧ { ⎨ { ⎩ 𝑝 ≤ 𝑝𝑑 𝑝 > 𝑝𝑑 (107.15) Where the current equivalent fracture strain 𝑝𝑓 = 𝑝𝑓 (𝜎 ∗, 𝑝̇∗, 𝑇∗) is defined as 𝑝𝑓 = [𝐷1 + 𝐷2exp(𝐷3𝜎 ∗)](1 + 𝑝̇∗)𝐷4(1 + 𝐷5𝑇∗) (107.16) and 𝐷1, 𝐷2, 𝐷3, 𝐷4, 𝐷5, 𝐷𝐶, 𝑝𝑑 are material parameters; the normalized equivalent plastic strain rate 𝑝̇∗ is defined by 𝑝̇∗ = 𝑝̇ 𝜀̇0 and the stress triaxiality 𝜎 ∗ reads 𝜎 ∗ = 𝜎𝐻 𝜎eq , 𝜎𝐻 = 𝑡𝑟(σ) 2.The Cockcroft-Latham damage evolution rule: 𝐷̇ = 𝐷𝐶 𝑊𝐶 max(𝜎1, 0)𝑝̇ where 𝐷𝐶, 𝑊𝐶 are material parameters. (107.17) (107.18) (107.19) Adiabatic heating is calculated as 𝑇̇ = 𝜒 𝛔: 𝐝𝑝 𝜌𝐶𝑝 = 𝜒 𝜎̃𝑒𝑞𝑟 ̇ 𝜌𝐶𝑝 (107.20) Where 𝜒 is the Taylor-Quinney parameter, 𝜌 is the density and 𝐶𝑝 is the specific heat. The initial value of the temperature 𝑇0 may be specified by the user. Element erosion occurs when one of the following several criteria are fulfilled: 1. The damage is greater than the critical value 𝐷 ≥ 𝐷𝐶 (107.21) 2. The maximum shear stress is greater than a critical value 𝜏max = max{|𝜎1 − 𝜎2|, ∣𝜎2 − 𝜎3∣, ∣𝜎3 − 𝜎1∣} ≥ 𝜏𝐶 (107.22) 3. The temperature is greater than a critical value 𝑇 ≥ 𝑇𝐶 (107.23) History Variable Description 1 2 3 4 5 8 9 Evaluation of damage D Evaluation of stress triaxiality 𝜎 ∗ Evaluation of damaged plastic strain r Evaluation of temperature T Evaluation of damaged plastic strain rate 𝑟 ̇ Evaluation of plastic work per volume W Evaluation of maximum shear stress 𝜏max *MAT_ORTHO_ELASTIC_PLASTIC This is Material Type 108. This model combines orthotropic elastic plastic behavior with an anisotropic yield criterion. This model is implemented only for shell elements. Card 1 1 Variable MID 2 RO Type A8 F Card 2 1 Variable SIGMA0 Type F Card 3 1 2 LC I 2 3 4 5 6 7 8 E11 E22 G12 PR12 PR23 PR31 F 3 F 4 F 5 F 6 F 7 F 8 QR1 CR1 QR2 CR2 F 3 F 4 F 5 F 6 7 8 Variable R11 R22 R33 R12 Type F Card 4 1 F 2 Variable AOPT BETA Type F F Card 5 Variable 1 XP Type F 2 YP F F 3 3 ZP F F 4 4 A1 F 5 6 7 8 7 8 5 A2 F 6 A3 Variable 1 V1 Type F 2 V2 F 3 V3 F 4 D17 F 5 D2 F 6 D3 F VARIABLE DESCRIPTION *MAT_108 7 8 MID RO E11 E22 G12 PR12 PR23 PR31 LC Material identification. A unique number or label not exceeding 8 characters must be specified. Mass Density Young’s Modulus in 11-direction Young’s Modulus in 22-direction Shear modulus in 12-direction Poisson’s ratio 12 Poisson’s ratio 23 Poisson’s ratio 31 Load curve ID. This curve defines effective stress versus effective plastic strain. QR1, CR1, QR2, and CR2 are ignored if LC is defined. SIGMA0 Initial yield stress, 𝜎0 QR1 CR1 QR2 CR2 R11 R22 R33 R12 Isotropic hardening parameter, 𝑄𝑅1 Isotropic hardening parameter, 𝐶𝑅1 Isotropic hardening parameter, 𝑄𝑅2 Isotropic hardening parameter, 𝐶𝑅2 Yield criteria parameter, 𝑅11 Yield criteria parameter, 𝑅22 Yield criteria parameter, 𝑅33 Yield criteria parameter, 𝑅12 AOPT *MAT_ORTHO_ELASTIC_PLASTIC DESCRIPTION Material axes option EQ.0.0: Locally orthotropic with material axes determined by element nodes as shown in Figure M2-1. Nodes 1, 2 and 4 of an element are identical to the node used for the definition of a coordinate system as by *DEFINE_- COORDINATE_NODES, and then rotated about the shell element normal by an angle BETA. EQ.2.0: Globally orthotropic with material axes determined by vectors defined below, as with *DEFINE_COORDI- NATE_VECTOR. EQ.3.0: Locally orthotropic material axes determined by offsetting the material axes by an angle, BETA, from a line determined by taking the cross product of the vec- tor v with the normal to the plane of the element. LT.0.0: the absolute value of AOPT is a coordinate system ID number (CID on *DEFINE_COORDINATE_NODES, *DEFINE_COORDINATE_SYSTEM or *DEFINE_CO- ORDINATE_VECTOR). Available in R3 version of 971 and later. BETA Material angle in degrees for AOPT = 0 and 3. BETA may be overridden on the element card, see *ELEMENT_SHELL_BETA. XP YP ZP Coordinates of point 𝐩 for AOPT = 1. A1 A2 A3 Components of vector 𝐚 for AOPT = 2. V1 V2 V3 Components of vector 𝐯 for AOPT = 3. D1 D2 D3 Components of vector 𝐝 for AOPT = 2. Remarks: The yield function is defined as where the equivalent stress 𝜎eq is defined as an anisotropic yield criterion 𝑓 = 𝑓 ̅(σ) − [𝜎0 + 𝑅(𝜀𝑝)] 𝜎eq = √𝐹(𝜎22 − 𝜎33)2 + 𝐺(𝜎33 − 𝜎11)2 + 𝐻(𝜎11 − 𝜎22)2 + 2𝐿𝜎23 2 + 2𝑀𝜎31 2 2 + 2𝑁𝜎12 Where F, G, H, L, M and N are constants obtained by test of the material in different orientations. They are defined as 𝐹 = 𝐺 = 𝐻 = 𝐿 = 𝑀 = 𝑁 = ( ( ( 2 + 𝑅22 2 + 𝑅33 2 + 𝑅11 2 − 𝑅33 2 − 𝑅11 2 − 𝑅22 2 ) 𝑅11 2 ) 𝑅22 2 ) 𝑅33 2 2𝑅23 2 2𝑅31 2 2𝑅12 The yield stress ratios are defined as follows 𝑅11 = 𝑅22 = 𝑅33 = 𝑅12 = 𝑅23 = 𝑅31 = 𝜎̅̅̅̅̅11 𝜎0 𝜎̅̅̅̅̅22 𝜎0 𝜎̅̅̅̅̅33 𝜎0 𝜎̅̅̅̅̅12 𝜏0 𝜎̅̅̅̅̅23 𝜏0 𝜎̅̅̅̅̅31 𝜏0 where 𝜎𝑖𝑗 is the measured yield stress values, 𝜎0 is the reference yield stress and 𝜏0 = 𝜎0/√3. The strain hardening is either defined by the load curve or the strain hardening R is defined by the extended Voce law, 𝑅(𝜀𝑝) = ∑ 𝑄𝑅𝑖[1 − exp(−𝐶𝑅𝑖𝜀𝑝)] 𝑖=1 where 𝜀𝑝 is the effective (or accumulated) plastic strain, and 𝑄𝑅𝑖 and 𝐶𝑅𝑖 are strain hardening parameters. *MAT_JOHNSON_HOLMQUIST_CERAMICS This is Material Type 110. This Johnson-Holmquist Plasticity Damage Model is useful for modeling ceramics, glass and other brittle materials. A more detailed description can be found in a paper by Johnson and Holmquist [1993]. Card 1 1 Variable MID Type A8 Card 2 1 Variable EPSI Type F Card 3 Variable 1 D1 Type F VARIABLE MID 2 RO F 2 T F 2 D2 F 3 G F 3 4 A F 4 5 B F 5 6 C F 6 7 M F 7 8 N F 8 SFMAX HEL PHEL BETA F F F F 3 K1 F 4 K2 F 5 K3 F 6 FS F DESCRIPTION 7 8 Material identification. A unique number or label not exceeding 8 characters must be specified. RO Density G A B C M Shear modulus Intact normalized strength parameter Fractured normalized strength parameter Strength parameter (for strain rate dependence) Fractured strength parameter (pressure exponent) VARIABLE DESCRIPTION N EPS0 T SFMAX HEL PHEL BETA D1 D2 K1 K2 K3 FS Intact strength parameter (pressure exponent). Quasi-static threshold strain rate. See *MAT_015. Maximum tensile pressure strength. Maximum normalized fractured strength (defaults to 1020 when set to 0.0). Hugoniot elastic limit. Pressure component at the Hugoniot elastic limit. Fraction of elastic energy loss converted to hydrostatic energy (affects bulking pressure (history variable 1) that accompanies damage). Parameter for plastic strain to fracture. Parameter for plastic strain to fracture (exponent). First pressure coefficient (equivalent to the bulk modulus). Second pressure coefficient. Third pressure coefficient. Element deletion criterion. FS.LT.0: fail if 𝑝∗ + 𝑡∗ < 0 (tensile failure). FS.EQ.0: no failure (default). FS.GT.0: fail if the effective plastic strain > FS. Remarks: The equivalent stress for a ceramic-type material is given by 𝜎 ∗ = 𝜎𝑖 ∗ − 𝐷(𝜎𝑖 ∗ − 𝜎𝑓 ∗) where ∗ = 𝑎(𝑝∗ + 𝑡∗)𝑛(1 + 𝑐ln𝜀̇∗) 𝜎𝑖 represents the intact, undamaged behavior. The superscript, '*', indicates a normalized quantity. The stresses are normalized by the equivalent stress at the Hugoniot elastic limit, the pressures are normalized by the pressure at the Hugoniot elastic limit, and the strain rate by the reference strain rate defined in the input. In this equation 𝑎 is the intact normalized strength parameter, 𝑐 is the strength parameter for strain rate dependence, 𝜀̇∗ is the normalized plastic strain rate, and, 𝑡∗ = 𝑝∗ = PHEL PHEL , , where 𝑇 is the maximum tensile pressure strength, PHEL is the pressure component at the Hugoniot elastic limit, and p is the pressure. 𝐷 = ∑ Δ𝜀𝑝 𝑝 𝜀𝑓 represents the accumulated damage (history variable 2) based upon the increase in plastic strain per computational cycle and the plastic strain to fracture and 𝑝 = 𝑑1(𝑝∗ + 𝑡∗)𝑑2 𝜀𝑓 ∗ = 𝑏(𝑝∗)𝑚(1 + 𝑐 ln𝜀̇) ≤ SFMAX 𝜎𝑓 represents the damaged behavior. The parameter d1 controls the rate at which damage accumulates. If it is made 0, full damage occurs in one time step i.e. instantaneously. It is also the best parameter to vary if one attempts to reproduce results generated by another finite element program. In undamaged material, the hydrostatic pressure is given by in compression and 𝑃 = 𝑘1𝜇 + 𝑘2𝜇2 + 𝑘3𝜇3 𝑃 = 𝑘1𝜇 ⁄ in tension where 𝜇 = 𝜌 𝜌0 − 1 . When damage starts to occur, there is an increase in pressure. A fraction, between 0 and 1, of the elastic energy loss, 𝛽, is converted into hydrostatic potential energy (pressure). The details of this pressure increase are given in the reference. Given HEL and G, 𝜇hel can be found iteratively from 2 + 𝑘3𝜇hel and, subsequently, for normalization purposes, HEL = 𝑘1𝜇hel + 𝑘2𝜇hel 3 + (4 3⁄ )𝑔(𝜇hel/(1 + 𝜇hel) 2-576 (EOS) LS-DYNA R10.0 𝑃hel = 𝑘1𝜇hel + 𝑘2𝜇hel and These are calculated automatically by LS-DYNA if 𝜌𝑓0 is zero on input. 𝜎hel = 1.5(hel − 𝑝hel) *MAT_JOHNSON_HOLMQUIST_CONCRETE This is Material Type 111. This model can be used for concrete subjected to large strains, high strain rates and high pressures. The equivalent strength is expressed as a function of the pressure, strain rate, and damage. The pressure is expressed as a function of the volumetric strain and includes the effect of permanent crushing. The damage is accumulated as a function of the plastic volumetric strain, equivalent plastic strain and pressure. A more detailed description of this model can be found in the paper by Holmquist, Johnson, and Cook [1993]. Card 1 1 Variable MID Type A8 Card 2 Variable Type Card 3 Variable 1 T F 1 D1 Type F VARIABLE MID 2 RO F 2 3 G F 3 4 A F 4 EPS0 EFMIN SFMAX F F F 2 D2 F 3 K1 F 4 K2 F 5 B F 5 PC F 5 K3 F 6 C F 6 UC F 6 FS F 7 N F 7 PL F 7 8 FC F 8 UL F 8 DESCRIPTION Material identification. A unique number or label not exceeding 8 characters must be specified. RO Mass density. G A B Shear modulus. Normalized cohesive strength. Normalized pressure hardening. VARIABLE DESCRIPTION C N FC T Strain rate coefficient. Pressure hardening exponent. Quasi-static uniaxial compressive strength. Maximum tensile hydrostatic pressure. EPS0 Quasi-static threshold strain rate. See *MAT_015. EFMIN Amount of plastic strain before fracture. SFMAX Normalized maximum strength. PC UC PL UL D1 D2 K1 K2 K3 FS Crushing pressure. Crushing volumetric strain. Locking pressure. Locking volumetric strain. Damage constant. Damage constant. Pressure constant. Pressure constant. Pressure constant. Failure type: FS.LT.0: fail if damage strength < 0 FS.EQ.0: fail if 𝑃∗ + 𝑇∗ ≤ 0 (tensile failure). FS.GT.0: fail if the effective plastic strain > FS. Remarks: The normalized equivalent stress is defined as 𝑓′𝑐 𝜎 ∗ = where 𝜎 is the actual equivalent stress, and 𝑓′ is the quasi-static uniaxial compressive strength. The expression is defined as: 𝜎 ∗ = [𝐴(1 − 𝐷) + 𝐵𝑃∗𝑁][1 + 𝐶ln(𝜀̇∗)] where 𝐷 is the damage parameter, 𝑃∗ = 𝑃 𝑓′𝑐⁄ is the normalized pressure and 𝜀̇∗ = 𝜀̇ 𝜀̇0⁄ is the dimensionless strain rate. The model incrementally accumulates damage, D, both from equivalent plastic strain and plastic volumetric strain, and is expressed as 𝐷 = ∑ Δ𝜀𝑝 + Δ𝜇𝑝 𝐷1(𝑃∗ + 𝑇∗)𝐷2 where Δ𝜀𝑝 and Δ𝜇𝑝 are the equivalent plastic strain and plastic volumetric strain, 𝐷1and 𝐷2 are material constants and 𝑇∗ = 𝑇 𝑓c ′⁄ is the normalized maximum tensile hydrostatic pressure. The damage strength, DS, is defined in compression when 𝑃∗ > 0 as DS = 𝑓𝑐 ′ min[SFMAX, 𝐴(1 − 𝐷) + 𝐵𝑃∗𝑁 ] [1 + 𝐶 ∗ ln(𝜀̇∗)] or in tension if 𝑃∗ < 0, as DS = 𝑓𝑐 ′ max [0, 𝐴(1 − 𝐷) − 𝐴 ( )] [1 + 𝐶 ∗ ln(𝜀̇∗)] 𝑃∗ The pressure for fully dense material is expressed as 𝑃 = 𝐾1𝜇̅̅̅̅ + 𝐾2𝜇̅̅̅̅2 + 𝐾3𝜇̅̅̅̅3 where 𝐾1 , 𝐾2 and 𝐾3 are material constants and the modified volumetric strain is defined as where 𝜇lock is the locking volumetric strain. 𝜇̅̅̅̅ = 𝜇 − 𝜇lock 1 + 𝜇lock *MAT_FINITE_ELASTIC_STRAIN_PLASTICITY This is Material Type 112. An elasto-plastic material with an arbitrary stress versus strain curve and arbitrary strain rate dependency can be defined. The elastic response of this model uses a finite strain formulation so that large elastic strains can develop before yielding occurs. This model is available for solid elements only. See Remarks below. Card 1 1 Variable MID 2 RO Type A8 F 3 E F 4 PR F 5 6 7 8 SIGY ETAN F F Default none none none none none 0.0 Card 2 Variable Type Default 1 C F 0 Card 3 1 2 P F 0 2 3 4 5 6 7 8 LCSS LCSR F 0 3 F 0 4 5 6 7 8 Variable EPS1 EPS2 EPS3 EPS4 EPS5 EPS6 EPS7 EPS8 Type Default F 0 F 0 F 0 F 0 F 0 F 0 F 0 F Card 4 1 2 3 4 5 6 7 8 Variable ES1 ES2 ES3 ES4 ES5 ES6 ES7 ES8 Type Default F 0 F 0 F 0 F 0 F 0 F 0 F 0 F 0 VARIABLE DESCRIPTION MID RO E PR SIGY ETAN C P LCSS Material identification. A unique number or label not exceeding 8 characters must be specified. Mass density. Young’s modulus. Poisson’s ratio. Yield stress. Tangent modulus, ignored if (LCSS.GT.0) is defined. Strain rate parameter, C, see formula below. Strain rate parameter, P, see formula below. Load curve ID or Table ID. Load curve ID defining effective stress versus effective plastic strain. If defined EPS1 - EPS8 and ES1 - ES8 are ignored. The table ID defines for each strain rate value a load curve ID giving the stress versus effective plastic strain for that rate, See Figure M24-1. The stress versus effective plastic strain curve for the lowest value of strain rate is used if the strain rate falls below the minimum value. Likewise, the stress versus effective plastic strain curve for the highest value of strain rate is used if the strain rate exceeds the maximum value. The strain rate parameters: C and P; the curve ID, LCSR; EPS1 - EPS8 and ES1 - ES8 are ignored if a Table ID is defined. LCSR Load curve ID defining strain rate scaling effect on yield stress. VARIABLE EPS1 - EPS8 DESCRIPTION Effective plastic strain values (optional if SIGY is defined). At least 2 points should be defined. The first point must be zero corresponding to the initial yield stress. WARNING: If the first point is nonzero the yield stress is extrapolated to determine the initial yield. If this option is used SIGY and ETAN are ignored and may be input as zero. ES1 - ES8 Corresponding yield stress values to EPS1 - EPS8. Remarks: The stress strain behavior may be treated by a bilinear stress strain curve by defining the tangent modulus, ETAN. Alternately, a curve similar to that shown in Figure M10-1 is expected to be defined by (EPS1,ES1) - (EPS8,ES8); however, an effective stress versus effective plastic strain curve (LCSS) may be input instead if eight points are insufficient. The cost is roughly the same for either approach. The most general approach is to use the table definition (LCSS) discussed below. Three options to account for strain rate effects are possible. 1. Strain rate may be accounted for using the Cowper and Symonds model which scales the yield stress with the factor 1 + ( 𝑝⁄ ) 𝜀̇ where 𝜀̇ is the strain rate, 𝜀̇ = √𝜀̇𝑖𝑗𝜀̇𝑖𝑗. 2. For complete generality a load curve (LCSR) to scale the yield stress may be input instead. In this curve the scale factor versus strain rate is defined. 3. If different stress versus strain curves can be provided for various strain rates, the option using the reference to a table (LCSS) can be used. Then the table input in *DEFINE_TABLE has to be used, see Figure M24-1. *MAT_TRIP This is Material Type 113. This isotropic elasto-plastic material model applies to shell elements only. It features a special hardening law aimed at modelling the temperature dependent hardening behavior of austenitic stainless TRIP-steels. TRIP stands for Transformation Induced Plasticity. A detailed description of this material model can be found in Hänsel, Hora, and Reissner [1998] and Schedin, Prentzas, and Hilding [2004]. Card 1 1 Variable MID 2 RO Type A8 F Default Card 2 Variable Type Default 1 A F 2 B F Card 3 1 2 Variable AHS BHS 3 E F 3 C 3 M 4 PR 5 CP 6 T0 7 8 TREF TA0 4 D 4 N 5 P 6 Q 7 8 E0MART VM0 5 6 EPS0 HMART 7 K1 8 K2 Type Default VARIABLE MID DESCRIPTION Material identification. A unique number or label not exceeding 8 characters must be specified. RO Mass density. E PR CP T0 TREF TA0 A B C D P Q *MAT_113 DESCRIPTION Young’s modulus. Poisson’s ratio. Adiabatic temperature calculation option: EQ.0.0: Adiabatic temperature calculation is disabled. GT.0.0: CP is the specific heat Cp. Adiabatic temperature calculation is enabled. Initial temperature T0 of the material if adiabatic temperature calculation is enabled. Reference temperature for output of the yield stress as history variable 1. Reference temperature TA0, the absolute zero for the used temperature scale, e.g. -273.15 if the Celsius scale is used and 0.0 if the Kelvin scale is used. Martensite rate equation parameter A, see equations below. Martensite rate equation parameter B, see equations below. Martensite rate equation parameter C, see equations below. Martensite rate equation parameter D, see equations below. Martensite rate equation parameter p, see equations below. Martensite rate equation parameter Q, see equations below. E0MART Martensite rate equation parameter E0(mart) , see equations below. VM0 The initial volume fraction of martensite 0.0 < Vm0 < 1.0 may be initialised using two different methods: GT.0.0: Vm0 is set to VM0. LT.0.0: Can be used only when there are initial plastic strains εp present, e.g. when using *INITIAL_STRESS_- SHELL. The absolute value of VM0 is then the load curve ID for a function f that sets 𝑉𝑚0 = 𝑓 (𝜀𝑝). The function f must be a monotonically nondecreasing function of 𝜀𝑝. DESCRIPTION *MAT_TRIP AHS BHS M N Hardening law parameter AHS, see equations below. Hardening law parameter BHS, see equations below. Hardening law parameter m, see equations below. Hardening law parameter n, see equations below. EPS0 Hardening law parameter ε0, see equations below. HMART Hardening law parameter ΔHγ→α’ , see equations below. Hardening law parameter K1, see equations below. Hardening law parameter K2, see equations below. K1 K2 Remarks: Here a short description is given of the TRIP-material model. The material model uses the von Mises yield surface in combination with isotropic hardening. The hardening is temperature dependent and therefore this material model must be run either in a coupled thermo-mechanical solution, using prescribed temperatures or using the adiabatic temperature calculation option. Setting the parameter CP to the specific heat Cp of the material activates the adiabatic temperature calculation that calculates the temperature rate from the equation 𝜎𝑖𝑗𝐷𝑖𝑗 𝜌𝐶𝑝 , 𝑇̇ = ∑ 𝑖,𝑗 where 𝛔: 𝐃𝑝 (the numerator) is the plastically dissipated heat. Using the Kelvin scale is recommended, even though other scales may be used without problems. The hardening behavior is described by the following equations. The Martensite rate equation is ∂𝑉𝑚 ∂𝜀̅𝑝 = ⎧0 {{ ⎨ {{ ⎩ 𝑝 ( 𝑉𝑚 1 − 𝑉𝑚 𝑉𝑚 where ) 𝐵+1 𝐵 [1 − tanh(C + D × 𝑇)] 𝜀 < 𝐸0(mart) exp ( 𝑇 − 𝑇𝐴0 ) 𝜀̅𝑝 ≥ 𝐸0(mart) 𝜀̅𝑝 = effective plastic strain and 𝑇 = temperature. The martensite fraction is integrated from the above rate equation: 𝑉𝑚 = ∫ ∂𝑉𝑚 ∂𝜀̅𝑝 𝑑𝜀̅𝑝. It always holds that 0.0 < Vm < 1.0. The initial martensite content is Vm0 and must be greater than zero and less than 1.0. Note that Vm0 is not used during a restart or when initializing the Vm history variable using *INITIAL_STRESS_SHELL. The yield stress σy is 𝜎𝑦 = {𝐵𝐻𝑆 − (𝐵𝐻𝑆 − 𝐴𝐻𝑆)exp(−𝑚[𝜀̅𝑝 + 𝜀0]𝑛)}(𝐾1 + 𝐾2𝑇) + Δ𝐻𝛾→𝛼′𝑉𝑚. The parameters p and B should fulfill the following condition 1 + 𝐵 < 𝑝 if not fulfilled then the martensite rate will approach infinity as 𝑉𝑚 approaches zero. Setting the parameter 𝜀0 larger than zero, typical range 0.001-0.02 is recommended. A part from the effective true strain a few additional history variables are output, see below. History variables that are output for post-processing: Variable Description 1 2 3 Yield stress of material at temperature TREF. Useful to evaluate the strength of the material after e.g., a simulated forming operation. Volume fraction martensite, Vm CP.EQ.0.0: Not used CP.GT.0.0: Temperature from adiabatic temperature calculation *MAT_LAYERED_LINEAR_PLASTICITY This is Material Type 114. A layered elastoplastic material with an arbitrary stress versus strain curve and an arbitrary strain rate dependency can be defined. This material must be used with the user defined integration rules, see *INTEGRATION- SHELL, for modeling laminated composite and sandwich shells where each layer can be represented by elastoplastic behavior with constitutive constants that vary from layer to layer. Lamination theory is applied to correct for the assumption of a uniform constant shear strain through the thickness of the shell. Unless this correction is applied, the stiffness of the shell can be grossly incorrect leading to poor results. Generally, without the correction the results are too stiff. This model is available for shell elements only. Also, see Remarks below. Card 1 1 Variable MID 2 RO Type A8 F 3 E F 4 PR F 5 6 7 8 SIGY ETAN FAIL TDEL F F F Default none none none none none 0.0 10.E+20 Card 2 Variable Type Default 1 C F 0 Card 3 1 2 P F 0 2 3 4 5 6 7 LCSS LCSR F 0 3 F 0 4 5 6 7 8 Variable EPS1 EPS2 EPS3 EPS4 EPS5 EPS6 EPS7 EPS8 Type Default F 0 F 0 F 0 F 0 F 0 F 0 F 0 F 0 2-588 (EOS) LS-DYNA R10.0 Card 4 1 2 3 4 5 6 7 8 Variable ES1 ES2 ES3 ES4 ES5 ES6 ES7 ES8 Type Default F 0 F 0 F 0 F 0 F 0 F 0 F 0 F 0 VARIABLE DESCRIPTION MID RO E PR SIGY ETAN FAIL Material identification. A unique number or label not exceeding 8 characters must be specified. Mass density. Young’s modulus. Poisson’s ratio. Yield stress. Tangent modulus, ignored if (LCSS.GT.0) is defined. Failure flag. LT.0.0: User defined failure subroutine, matusr_24 in dyn21.F, is called to determine failure EQ.0.0: Failure is not considered. This option is recommended if failure is not of interest since many calculations will be saved. GT.0.0: Plastic strain to failure. When the plastic strain reaches this value, the element is deleted from the calculation. TDEL Minimum time step size for automatic element deletion. C P Strain rate parameter, C, see formula below. Strain rate parameter, P, see formula below. LCSS *MAT_LAYERED_LINEAR_PLASTICITY DESCRIPTION Load curve ID or Table ID. Load curve ID defining effective stress versus effective plastic strain. If defined EPS1 - EPS8 and ES1 - ES8 are ignored. The table ID defines for each strain rate value a load curve ID giving the stress versus effective plastic strain for that rate, See Figure M24-1. The stress versus effective plastic strain curve for the lowest value of strain rate is used if the strain rate falls below the minimum value. Likewise, the stress versus effective plastic strain curve for the highest value of strain rate is used if the strain rate exceeds the maximum value. The strain rate parameters: C and P; the curve ID, LCSR; EPS1 - EPS8 and ES1 - ES8 are ignored if a Table ID is defined. LCSR Load curve ID defining strain rate scaling effect on yield stress. EPS1 - EPS8 Effective plastic strain values (optional if SIGY is defined). At least 2 points should be defined. The first point must be zero corresponding to the initial yield stress. WARNING: If the first point is nonzero the yield stress is extrapolated to determine the initial yield. If this option is used SIGY and ETAN are ignored and may be input as zero. ES1 - ES8 Corresponding yield stress values to EPS1 - EPS8. Remarks: The stress strain behavior may be treated by a bilinear stress strain curve by defining the tangent modulus, ETAN. Alternately, a curve similar to that shown in Figure M10-1 is expected to be defined by (EPS1, ES1) - (EPS8, ES8); however, an effective stress versus effective plastic strain curve (LCSS) may be input instead if eight points are insufficient. The cost is roughly the same for either approach. The most general approach is to use the table definition (LCSS) discussed below. Three options to account for strain rate effects are possible. 1. Strain rate may be accounted for using the Cowper and Symonds model which scales the yield stress with the factor 1 + ( 𝑝⁄ ) 𝜀̇ where 𝜀̇ is the strain rate, 𝜀̇ = √𝜀̇𝑖𝑗𝜀̇𝑖𝑗. 2. For complete generality a load curve (LCSR) to scale the yield stress may be input instead. In this curve the scale factor versus strain rate is defined. 3. If different stress versus strain curves can be provided for various strain rates, the option using the reference to a table (LCSS) can be used. Then the table input in *DEFINE_TABLE has to be used, see Figure M24-1. *MAT_UNIFIED_CREEP This is Material Type 115. This is an elastic creep model for modeling creep behavior when plastic behavior is not considered. Card 1 1 Variable MID 2 RO Type A8 F 3 E F 4 PR F 5 A F 6 N F 7 M F 8 Default none none none none none none none VARIABLE MID DESCRIPTION Material identification. A unique number or label not exceeding 8 characters must be specified. RO E PR A N M Mass density. Young’s modulus. Poisson’s ratio. Stress coefficient. Stress exponent. Time exponent. Remarks: The effective creep strain, 𝜀̅𝑐, given as: 𝜀̅𝑐 = 𝐴𝜎̅̅̅̅̅ 𝑛𝑡 ̅𝑚 where A, n, and m are constants and 𝑡 ̅ is the effective time. The effective stress, 𝜎̅̅̅̅̅, is defined as: 𝜎̅̅̅̅̅ = √ 𝜎𝑖𝑗𝜎𝑖𝑗 The creep strain, therefore, is only a function of the deviatoric stresses. The volumetric behavior for this material is assumed to be elastic. By varying the time constant m primary creep (m < 1), secondary creep (m = 1), and tertiary creep (m > 1) can be modeled. This model is described by Whirley and Henshall [1992]. *MAT_UNIFIED_CREEP This is Material Type 115_O. This is an orthotropic elastic creep model for modeling creep behavior when plastic behavior is not considered. This material is only available for solid elements, and is available for both explicit and implicit dynamics. Card 1 1 Variable MID 2 RO Type A8 F 3 E1 F 4 E2 F 5 E3 F 6 7 8 PR21 PR31 PR32 F F F Default none none none none none none none none Card 2 1 2 3 Variable G12 G23 G13 Type F F F 4 A F 5 N F 6 M F 7 8 Default none none none none none none Card 3 1 2 Variable AOPT MACF Type F F 3 XP F 4 YP F 5 ZP F 6 A1 F 7 A2 F 8 A3 F Default none none none none none none none none Card 4 Variable 1 V1 Type F 2 V2 F 3 V3 F 4 D1 F 5 D2 F 6 D3 F 7 8 Default none none none none none none VARIABLE DESCRIPTION MID RO Ei PRij Gij A N M Material identification. A unique number or label not exceeding 8 characters must be specified. Mass density. Young’s moduli. Elastic Poisson’s ratios. Elastic shear moduli. Stress coefficient. Stress exponent. Time exponent. AOPT *MAT_UNIFIED_CREEP DESCRIPTION Material axes option : EQ.0.0: locally orthotropic with material axes determined by element nodes 1, 2, and 4, as with *DEFINE_COORDI- NATE_NODES. EQ.1.0: locally orthotropic with material axes determined by a point in space and the global location of the element center; this is the a-direction. This option is for solid elements only. EQ.2.0: globally orthotropic with material axes determined by vectors defined below, as with *DEFINE_COORDI- NATE_VECTOR. EQ.3.0: locally orthotropic material axes determined by rotating the material axes about the element normal by an angle, BETA, from a line in the plane of the element defined by the cross product of the vector v with the element normal. EQ.4.0: locally orthotropic in cylindrical coordinate system with the material axes determined by a vector v, and an originating point, p, which define the centerline ax- is. This option is for solid elements only. LT.0.0: the absolute value of AOPT is a coordinate system ID number (CID on *DEFINE_COORDINATE_NODES, *DEFINE_COORDINATE_SYSTEM or *DEFINE_CO- ORDINATE_VECTOR). Available in R3 version of 971 and later. MACF Material axes change flag for brick elements: EQ.1: No change, default, EQ.2: switch material axes a and b, EQ.3: switch material axes a and c, EQ.4: switch material axes b and c. XP, YP, ZP Define coordinates of point p for AOPT = 1 and 4. A1, A2, A3 Define components of vector a for AOPT = 2. V1, V2, V3 Define components of vector v for AOPT = 3 and 4. VARIABLE DESCRIPTION D1, D2, D3 Define components of vector d for AOPT = 2. BETA Material angle in degrees for AOPT = 3, may be overridden on the element card, see *ELEMENT_SHELL_BETA or *ELEMENT_- SOLID_ORTHO. Remarks: The stress-strain relationship is based on an additive split of the strain, Here, the multiaxial creep strain is given by 𝜺̇ = 𝜺̇𝑒 + 𝜺̇𝑐. and 𝜀̅𝑐 is the effective creep strain, 𝒔 the deviatoric stress 𝜺̇𝑐 = 𝜀̅𝑐̇ 2𝒔 3𝜎̅̅̅̅̅ , and 𝜎̅̅̅̅̅ the effective stress 𝒔 = 𝝈 − tr(𝝈)𝑰. 𝜎̅̅̅̅̅ = √ 𝒔: 𝒔. The effective creep strain is given by where A, N, and M are constants. The stress increment is given by 𝜀̅𝑐̇ = 𝐴𝜎̅̅̅̅̅ 𝑁𝑡𝑀, ∆𝝈 = 𝑪∆𝜺𝑒 = 𝑪(∆𝜺 − ∆𝜺𝑐), where the constitutive matrix 𝑪 is taken as orthotropic and can be represented in Voigt notation by its inverse as 𝑪−1 = 𝐸1 𝜐12 𝐸1 𝜐13 𝐸1 − − 𝜐21 𝐸2 𝐸2 𝜐23 𝐸2 − − 𝜐31 𝐸3 𝜐32 𝐸3 𝐸3 ⎤ ⎥ ⎥ ⎥ ⎥ ⎥ ⎥ ⎥ ⎥ . ⎥ ⎥ ⎥ ⎥ ⎥ ⎥ ⎥ ⎥ 𝐺13⎦ 𝐺12 𝐺23 − − ⎡ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎣ *MAT_116 This is Material Type 116. This material is for modeling the elastic responses of composite layups that have an arbitrary number of layers through the shell thickness. A pre-integration is used to compute the extensional, bending, and coupling stiffness for use with the Belytschko-Tsay resultant shell formulation. The angles of the local material axes are specified from layer to layer in the *SECTION_SHELL input. This material model must be used with the user defined integration rule for shells, see *IN- TEGRATION_SHELL, which allows the elastic constants to change from integration point to integration point. Since the stresses are not computed in the resultant formulation, the stresses output to the binary databases for the resultant elements are zero. Note that this shell does not use laminated shell theory and that storage is allocated for just one integration point (as reported in D3HSP) regardless of the layers defined in the integration rule. Card 1 1 Variable MID Type A8 Card 2 1 2 RO F 2 3 EA F 3 4 EB F 4 Variable GAB GBC GCA AOPT Type F F F F Card 3 Variable 1 XP Type F Card 4 Variable 1 V1 Type F LS-DYNA R10.0 2 YP F 2 V2 F 3 ZP F 3 V3 F 4 A1 F 4 D1 F 5 EC F 5 5 A2 F 5 D2 F 6 7 8 PRBA PRCA PRCB F 6 6 A3 F 6 D3 F F 7 F 8 7 8 7 8 BETA VARIABLE DESCRIPTION MID RO EA EB EC PRBA PRCA PRCB GAB GBC GCA Material identification. A unique number or label not exceeding 8 characters must be specified. Mass density. Ea, Young’s modulus in a-direction. Eb, Young’s modulus in b-direction. Ec, Young’s modulus in c-direction. ba, Poisson’s ratio ba. ca, Poisson’s ratio ca. cb, Poisson’s ratio cb. Gab, shear modulus ab. Gbc, shear modulus bc. Gca, shear modulus ca. VARIABLE DESCRIPTION AOPT Material axes option, see Figure M2-1: EQ.0.0: locally orthotropic with material axes determined by element nodes as shown in Figure M2-1. Nodes 1, 2, and 4 of an element are identical to the nodes used for the definition of a coordinate system as by *DEFINE_- COORDINATE_NODES, and then rotated about the shell element normal by an angle BETA. EQ.2.0: globally orthotropic with material axes determined by vectors defined below, as with *DEFINE_COORDI- NATE_VECTOR. EQ.3.0: locally orthotropic material axes determined by rotating the material axes about the element normal by an angle, BETA, from a line in the plane of the element defined by the cross product of the vector v with the element normal. LT.0.0: the absolute value of AOPT is a coordinate system ID number (CID on *DEFINE_COORDINATE_NODES, *DEFINE_COORDINATE_SYSTEM or *DEFINE_CO- ORDINATE_VECTOR). Available in R3 version of 971 and later. XP, YP, ZP Define coordinates of point p for AOPT = 1 and 4. A1, A2, A3 Define components of vector a for AOPT = 2. V1, V2, V3 Define components of vector v for AOPT = 3 and 4. D1, D2, D3 Define components of vector d for AOPT = 2. BETA Material angle in degrees for AOPT = 0 and 3, may be overridden on the element card, see *ELEMENT_SHELL_BETA. Remarks: This material law is based on standard composite lay-up theory. The implementation, [Jones 1975], allows the calculation of the force, N, and moment, M, stress resultants from: ⎧Nx ⎫ } { Ny ⎬ ⎨ } { Nxy⎭ ⎩ = 𝐴11 𝐴12 𝐴16 ⎤ ⎡ 𝐴21 𝐴22 𝐴26 ⎥ ⎢ 𝐴16 𝐴26 𝐴66⎦ ⎣ }}⎫ {{⎧𝜀𝑥 𝜀𝑦 }}⎬ {{⎨ 0⎭ 𝜀𝑧 ⎩ + 𝐵11 𝐵12 𝐵16 ⎤ ⎡ 𝐵21 𝐵22 𝐵26 ⎥ ⎢ 𝐵16 𝐵26 𝐵66⎦ ⎣ {⎧𝜅x }⎫ 𝜅y 𝜅z⎭}⎬ ⎩{⎨ ⎧ 𝑀𝑥 ⎫ } { My ⎬ ⎨ } { Mxy⎭ ⎩ = 𝐵11 𝐵12 𝐵16 ⎤ ⎡ 𝐵21 𝐵22 𝐵26 ⎥ ⎢ 𝐵16 𝐵26 𝐵66⎦ ⎣ }}⎫ {{⎧𝜀𝑥 𝜀𝑦 }}⎬ {{⎨ 0⎭ 𝜀𝑧 ⎩ + 𝐷11 𝐷12 𝐷16 ⎤ 𝐷21 𝐷22 𝐷26 ⎥ 𝐷16 𝐷26 𝐷66⎦ ⎡ ⎢ ⎣ {⎧𝜅x }⎫ 𝜅y 𝜅z⎭}⎬ ⎩{⎨ where 𝐴𝑖𝑗 is the extensional stiffness, 𝐷𝑖𝑗is the bending stiffness, and 𝐵𝑖𝑗 is the coupling stiffness which is a null matrix for symmetric lay-ups. The mid-surface stains and 0 and 𝜅𝑖𝑗respectively. Since these stiffness matrices are curvatures are denoted by 𝜀𝑖𝑗 symmetric, 18 terms are needed per shell element in addition to the shell resultants which are integrated in time. This is considerably less storage than would typically be required with through thickness integration which requires a minimum of eight history variables per integration point, e.g., if 100 layers are used 800 history variables would be stored. Not only is memory much less for this model, but the CPU time required is also considerably reduced. *MAT_117 This is Material Type 117. This material is used for modeling the elastic responses of composites where a pre-integration is used to compute the extensional, bending, and coupling stiffness coefficients for use with the Belytschko-Tsay resultant shell formulation. Since the stresses are not computed in the resultant formulation, the stresses output to the binary databases for the resultant elements are zero. NOTE: This material does not support specification of a ma- terial angle, 𝛽𝑖, for each through-thickness integra- tion point of a shell. Card 1 1 Variable MID Type A8 Card 2 1 2 RO F 2 3 4 5 6 7 8 3 4 5 6 7 8 Variable C11 C12 C22 C13 C23 C33 C14 C24 Type F Card 3 1 F 2 F 3 F 4 F 5 F 6 F 7 F 8 Variable C34 C44 C15 C25 C35 C45 C55 C16 Type F Card 4 1 F 2 F 3 F 4 F 5 F 6 F 7 F 8 Variable C26 C36 C46 C56 C66 AOPT Type F F F F F Variable 1 XP Type F Card 6 Variable 1 V1 Type F *MAT_COMPOSITE_MATRIX 2 YP F 2 V2 F 3 ZP F 3 V3 F 4 A1 F 4 D1 F 5 A2 F 5 D2 F 6 A3 F 6 D3 F 7 8 7 8 BETA F VARIABLE DESCRIPTION MID RO CIJ Material identification. A unique number or label not exceeding 8 characters must be specified. Mass density. 𝐶𝑖𝑗 coefficients of stiffness matrix in the material coordinate system. AOPT Material axes option, see Figure M2-1: EQ.0.0: locally orthotropic with material axes determined by element nodes as shown in Figure M2-1. Nodes 1, 2, and 4 of an element are identical to the nodes used for the definition of a coordinate system as by *DEFINE_- COORDINATE_NODES, and then rotated about the shell element normal by an angle BETA. EQ.2.0: globally orthotropic with material axes determined by vectors defined below, as with *DEFINE_COORDI- NATE_VECTOR. EQ.3.0: locally orthotropic material axes determined by rotating the material axes about the element normal by an angle, BETA, from a line in the plane of the element defined by the cross product of the vector 𝐯 with the element normal. LT.0.0: the absolute value of AOPT is a coordinate system ID number (CID on *DEFINE_COORDINATE_NODES, *DEFINE_COORDINATE_SYSTEM or *DEFINE_CO- VARIABLE DESCRIPTION ORDINATE_VECTOR). Available in R3 version of 971 and later. XP, YP, ZP Define coordinates of point 𝐩 for AOPT = 1 and 4. A1, A2, A3 Define components of vector 𝐚 for AOPT = 2. V1, V2, V3 Define components of vector 𝐯 for AOPT = 3 and 4. D1, D2, D3 Define components of vector 𝐝 for AOPT = 2. BETA Μaterial angle in degrees for AOPT = 0 and 3, may be overridden on the element card, see *ELEMENT_SHELL_BETA. Remarks: The calculation of the force, 𝑁𝑖𝑗, and moment, 𝑀𝑖𝑗, stress resultants is given in terms of the membrane strains, 𝜀𝑖 0, and shell curvatures 𝐶𝑖𝑗, 𝜅𝑖, as: 𝑁𝑥 ⎤ ⎡ 𝑁𝑦 ⎥ ⎢ ⎥ ⎢ 𝑁𝑥𝑦 ⎥ ⎢ ⎥ ⎢ 𝑀𝑥 ⎥ ⎢ ⎥ ⎢ 𝑀𝑦 ⎥ ⎢ 𝑀𝑥𝑦⎦ ⎣ = 𝐶11 𝐶12 𝐶13 𝐶14 𝐶15 𝐶16 ⎤ ⎡ 𝐶21 𝐶22 𝐶23 𝐶24 𝐶25 𝐶26 ⎥ ⎢ ⎥ ⎢ 𝐶31 𝐶32 𝐶33 𝐶34 𝐶35 𝐶36 ⎥ ⎢ ⎥ ⎢ 𝐶41 𝐶42 𝐶43 𝐶44 𝐶45 𝐶46 ⎥ ⎢ 𝐶51 𝐶52 𝐶53 𝐶54 𝐶55 𝐶56 ⎥ ⎢ 𝐶61 𝐶62 𝐶63 𝐶64 𝐶65 𝐶66⎦ ⎣ 𝜀𝑥 ⎤ ⎡ 𝜀𝑦 ⎥ ⎢ ⎥ ⎢ ⎥ ⎢ 𝜀𝑧 ⎥ ⎢ κ𝑥 ⎥ ⎢ 𝜅𝑦 ⎥ ⎢ κ𝑧⎦ ⎣ where 𝐶𝑖𝑗 = 𝐶𝑗𝑖. In this model this symmetric matrix is transformed into the element local system and the coefficients are stored as element history variables. In model type *MAT_COMPOSITE_DIRECT below, the resultants are already assumed to be given in the element local system which reduces the storage since the 21 coefficients are not stored as history variables as part of the element data. The shell thickness is built into the coefficient matrix and, consequently, within the part ID, which references this material ID, the thickness must be uniform. *MAT_COMPOSITE_DIRECT This is Material Type 118. This material is used for modeling the elastic responses of composites where a pre-integration is used to compute the extensional, bending, and coupling stiffness coefficients for use with the Belytschko-Tsay resultant shell formulation. Since the stresses are not computed in the resultant formulation, the stresses output to the binary databases for the resultant elements are zero. Card 1 1 Variable MID Type A8 Card 2 1 2 RO F 2 3 4 5 6 7 8 3 4 5 6 7 8 Variable C11 C12 C22 C13 C23 C33 C14 C24 Type F Card 3 1 F 2 F 3 F 4 F 5 F 6 F 7 F 8 Variable C34 C44 C15 C25 C35 C45 C55 C16 Type F Card 4 1 F 2 F 3 F 4 F 5 F 6 F 7 F 8 Variable C26 C36 C46 C56 C66 Type F F F F F VARIABLE MID DESCRIPTION Material identification. A unique number or label not exceeding 8 characters must be specified. RO Mass density. VARIABLE DESCRIPTION CIJ 𝐶𝑖𝑗coefficients of the stiffness matrix. Remarks: The calculation of the force, 𝑁𝑖𝑗, and moment, 𝑀𝑖𝑗, stress resultants is given in terms of the membrane strains, 𝜀𝑖 ⎫ 0, and shell curvatures, 𝜅𝑖, as: ⎧𝑁𝑥 𝑁𝑦 𝑁𝑥𝑦 𝑀𝑥 𝑀𝑦 𝑀𝑥𝑦⎭ 𝐶11 𝐶12 𝐶13 𝐶14 𝐶15 𝐶16 ⎤ ⎡ 𝐶21 𝐶22 𝐶23 𝐶24 𝐶25 𝐶26 ⎥ ⎢ ⎥ ⎢ 𝐶31 𝐶32 𝐶33 𝐶34 𝐶35 𝐶36 ⎥ ⎢ ⎥ ⎢ 𝐶41 𝐶42 𝐶43 𝐶44 𝐶45 𝐶46 ⎥ ⎢ 𝐶51 𝐶52 𝐶53 𝐶54 𝐶55 𝐶56 ⎥ ⎢ 𝐶61 𝐶62 𝐶63 𝐶64 𝐶65 𝐶66⎦ ⎣ {{{{{ {{{{{ }}}}} }}}}} = ⎬ ⎨ ⎩ ⎫ ⎧𝜀𝑥 𝜀𝑦 𝜀𝑧 𝜅𝑥 𝜅𝑦 𝜅𝑥𝑦⎭ }}}}} }}}}} {{{{{ {{{{{ ⎩ ⎨ ⎬ where 𝐶𝑖𝑗 = 𝐶𝑗𝑖. In this model the stiffness coefficients are already assumed to be given in the element local system which reduces the storage. Great care in the element orientation and choice of the local element system, see *CONTROL_ACCURACY, must be observed if this model is used. The shell thickness is built into the coefficient matrix and, consequently, within the part ID, which references this material ID, the thickness must be uniform. *MAT_GENERAL_NONLINEAR_6DOF_DISCRETE_BEAM This is Material Type 119. This is a very general spring and damper model. This beam Additional the MAT_SPRING_GENERAL_NONLINEAR option. is based on unloading options have been included. The two nodes defining the beam may be coincident to give a zero length beam, or offset to give a finite length beam. For finite length discrete beams the absolute value of the variable SCOOR in the SECTION_- BEAM input should be set to a value of 2.0 or 3.0 to give physically correct behavior. A triad is used to orient the beam for the directional springs. Card 1 1 Variable MID Type A8 Card 2 1 2 RO F 2 3 KT F 3 4 KR F 4 5 6 7 8 IUNLD OFFSET DAMPF IFLAG I 5 F 6 F 7 I 8 Variable LCIDTR LCIDTS LCIDTT LCIDRR LCIDRS LCIDRT Type I Card 3 1 I 2 I 3 I 4 I 5 I 6 7 8 Variable LCIDTUR LCIDTUS LCIDTUT LCIDRUR LCIDRUS LCIDRUT Type I Card 4 1 I 2 I 3 I 4 I 5 I 6 7 8 Variable LCIDTDR LCIDTDS LCIDTDT LCIDRDR LCIDRDS LCIDRDT Type I I I I I Card 5 1 2 3 4 5 6 7 8 Variable LCIDTER LCIDTES LCIDTET LCIDRER LCIDRES LCIDRET Type I Card 6 1 I 2 I 3 I 4 I 5 I 6 7 8 Variable UTFAILR UTFAILS UTFAILT WTFAILR WTFAILS WTFAILT Type F Card 7 1 F 2 F 3 F 4 F 5 F 6 7 8 Variable UCFAILR UCFAILS UCFAILT WCFAILR WCFAILS WCFAILT Type F Card 8 1 F 2 F 3 F 4 F 5 F 6 7 8 Variable IUR IUS IUT IWR IWS IWT Type F F F F F F VARIABLE DESCRIPTION MID RO KT KR Material identification. A unique number or label not exceeding 8 characters must be specified. Mass density, see also volume in *SECTION_BEAM definition. Translational stiffness for unloading option 2.0. Rotational stiffness for unloading option 2.0. DAMPF IFLAG *MAT_GENERAL_NONLINEAR_6DOF_DISCRETE_BEAM DESCRIPTION Damping factor for stability. Values in the neighborhood of unity are recommended. This damping factor is properly scaled to eliminate time step size dependency. Also, it is active if and only if the local stiffness is defined. Flag for switching between the displacement (default IFLAG = 0) and linear strain (IFLAG = 1) formulations. The displacement formulation is the one used in all other models. For the linear strain formulation, the displacements and velocities are divided by the initial length of the beam. IUNLD Unloading option (Also see Figure M119-1.): EQ.0.0: Loading and unloading follow loading curve EQ.1.0: Loading follows loading curve, unloading follows unloading curve. The unloading curve ID if undefined is taken as the loading curve. EQ.2.0: Loading follows loading curve, unloading follows unloading stiffness, KT or KR, to the unloading curve. The loading and unloading curves may only intersect at the origin of the axes. EQ.3.0: Quadratic unloading from peak displacement value to a permanent offset. OFFSET LCIDTR if the Offset factor between 0 and 1.0 to determine permanent set upon in unloading compression and tension are equal to the product of this offset value and the maximum compressive and tensile displacements, respectively. The permanent sets IUNLD = 3.0. Load curve ID defining translational force resultant along local r- axis versus relative translational displacement. If zero, no stiffness related forces are generated for this degree of freedom. The loading curves must be defined from the most negative displacement to the most positive displacement. The force does not need to increase monotonically. The curves in this input are linearly extrapolated when the displacement range falls outside the curve definition. LCIDTS Load curve ID defining translational force resultant along local s- axis versus relative translational displacement. VARIABLE LCIDTT LCIDRR LCIDRS LCIDRT LCIDTUR DESCRIPTION Load curve ID defining translational force resultant along local t- axis versus relative translational displacement. Load curve ID defining rotational moment resultant about local r- axis versus relative rotational displacement. Load curve ID defining rotational moment resultant about local s- axis versus relative rotational displacement. Load curve ID defining rotational moment resultant about local t- axis versus relative rotational displacement. this curve must force values defined by Load curve ID defining translational force resultant along local r- axis versus relative translational displacement during unloading. The increase monotonically from the most negative displacement to the most positive displacement. For IUNLD = 1.0, the slope of this curve must equal or exceed the loading curve for stability reasons. This is not the case for IUNLD = 2.0. For loading and unloading to follow the same path simply set LCIDTUR = LCIDTR. For options IUNLD = 0.0 or 3.0 the unloading curve is not required. For IUNLD = 2.0, if LCIDTUR is left blank or zero, the default is to use the same curve for unloading as for loading. LCIDTUS LCIDTUT LCIDRUR LCIDRUS LCIDRUT LCIDTDR LCIDTDS Load curve ID defining translational force resultant along local s- axis versus relative translational displacement during unloading. Load curve ID defining translational force resultant along local t- axis versus relative translational displacement during unloading. Load curve ID defining rotational moment resultant about local r- axis versus relative rotational displacement during unloading. Load curve ID defining rotational moment resultant about local s- axis versus relative rotational displacement during unloading. Load curve ID defining rotational moment resultant about local t- axis versus relative rotational displacement during unloading. If zero, no viscous forces are generated for this degree of freedom. Load curve ID defining translational damping force resultant along local r-axis versus relative translational velocity. Load curve ID defining translational damping force resultant along local s-axis versus relative translational velocity. LCIDTDT LCIDRDR LCIDRDS LCIDRDT LCIDTER LCIDTES LCIDTET LCIDRER LCIDRES LCIDRET UTFAILR UTFAILS UTFAILT WTFAILR *MAT_GENERAL_NONLINEAR_6DOF_DISCRETE_BEAM DESCRIPTION Load curve ID defining translational damping force resultant along local t-axis versus relative translational velocity. Load curve ID defining rotational damping moment resultant about local r-axis versus relative rotational velocity. Load curve ID defining rotational damping moment resultant about local s-axis versus relative rotational velocity. Load curve ID defining rotational damping moment resultant about local t-axis versus relative rotational velocity. Load curve ID defining translational damping force scale factor versus relative displacement in local r-direction. Load curve ID defining translational damping force scale factor versus relative displacement in local s-direction. Load curve ID defining translational damping force scale factor versus relative displacement in local t-direction. Load curve ID defining rotational damping moment resultant scale factor versus relative displacement in local r-rotation. Load curve ID defining rotational damping moment resultant scale factor versus relative displacement in local s-rotation. Load curve ID defining rotational damping moment resultant scale factor versus relative displacement in local t-rotation. Optional, translational displacement at failure in tension. If zero, the corresponding displacement, ur, is not considered in the failure calculation. Optional, translational displacement at failure in tension. If zero, the corresponding displacement, us, is not considered in the failure calculation. Optional, translational displacement at failure in tension. If zero, the corresponding displacement, ut, is not considered in the failure calculation. Optional, rotational displacement at failure in tension. If zero, the corresponding rotation, θr, is not considered in the failure calculation. VARIABLE WTFAILS WTFAILT UCFAILR UCFAILS UCFAILT WCFAILR WCFAILS WCFAILT IUR IUS IUT IWR IWS IWT DESCRIPTION Optional, rotational displacement at failure in tension. If zero, the corresponding rotation, θs, is not considered in the failure calculation. Optional rotational displacement at failure in tension. If zero, the corresponding rotation, θt, is not considered in the failure calculation. Optional, translational displacement at failure in compression. If zero, the corresponding displacement, ur, is not considered in the failure calculation. Define as a positive number. Optional, translational displacement at failure in compression. If zero, the corresponding displacement, us, is not considered in the failure calculation. Define as a positive number. Optional, translational displacement at failure in compression. If zero, the corresponding displacement, ut, is not considered in the failure calculation. Define as a positive number. Optional, rotational displacement at failure in compression. If zero, the corresponding rotation, θr, is not considered in the failure calculation. Define as a positive number. Optional, rotational displacement at failure in compression. If zero, the corresponding rotation, θs, is not considered in the failure calculation. Define as a positive number. Optional, rotational displacement at failure in compression. If zero, the corresponding rotation, θt, is not considered in the failure calculation. Define as a positive number. Initial translational displacement along local r-axis. Initial translational displacement along local s-axis. Initial translational displacement along local t-axis. Initial rotational displacement about the local r-axis. Initial rotational displacement about the local s-axis. Initial rotational displacement about the local t-axis. *MAT_GENERAL_NONLINEAR_6DOF_DISCRETE_BEAM Catastrophic failure, which is based on displacement resultants, occurs if either of the following inequalities are satisfied: ) ( 𝑢𝑟 tfail 𝑢𝑟 + ( 𝑢𝑠 tfail 𝑢𝑠 ) + ( 𝑢𝑡 tfail 𝑢𝑡 ) + ( 𝜃𝑟 tfail 𝜃𝑟 ) + ( ) + 𝜃𝑠 tfail 𝜃𝑠 ⎜⎛ 𝜃𝑡 𝑡𝑓𝑎𝑖𝑙 𝜃𝑡 ⎝ ⎟⎞ ⎠ ( 𝑢𝑟 cfail 𝑢𝑟 ) + ( 𝑢𝑠 cfail 𝑢𝑠 ) + ( 𝑢𝑡 cfail 𝑢𝑡 ) + ( 𝜃𝑟 cfail 𝜃𝑟 ) + ( 𝜃𝑠 cfail 𝜃𝑠 ) + ( 𝜃𝑡 cfail 𝜃𝑡 − 1. ≥ 0 ) − 1. ≥ 0 After failure the discrete element is deleted. If failure is included either the tension failure or the compression failure or both may be used. Unload = 0 Loading-unloading curve Unload = 2 Unloading curve DISPLACEMENT Unloading curve DISPLACEMENT Unload = 1 Unload = 3 DISPLACEMENT umin × OFFSET umin Quadratic unloading DISPLACEMENT Figure M119-1. Load and unloading behavior. There are two formulations for calculating the force. The first is the standard displacement formulation, where, for example, the force in a linear spring is 𝐹 = −𝐾Δℓ for a change in length of the beam of Δℓ. The second formulation is based on the linear strain, giving a force of 𝐹 = −𝐾 Δℓ ℓ0 for a beam with an initial length of ℓ0. This option is useful when there are springs of different lengths but otherwise similar construction since it automatically reduces the stiffness of the spring as the length increases, allowing an entire family of springs to be modeled with a single material. Note that all the displacement and velocity components are divided by the initial length, and therefore the scaling applies to the damping and rotational stiffness. *MAT_GURSON This is Material Type 120. This is the Gurson dilatational-plastic model. This model is available for shell and solid elements. A detailed description of this model can be found in the following references: Gurson [1975, 1977], Chu and Needleman [1980] and Tvergaard and Needleman [1984]. The implementation in LS-DYNA is based on the implementation of Feucht [1998] and Faßnacht [1999], which was recoded at LSTC. Strain rate dependency can be defined via a Table definition. Card 1 1 Variable MID 2 RO Type A8 F 3 E F 4 PR F 5 SIGY F 6 N F 7 Q1 F 8 Q2 F Default none none none none none 0.0 none none Card 2 Variable Type Default 1 FC F 0 Card 3 1 2 F0 F 0 2 3 EN F 0 3 4 SN F 0 4 5 FN F 0 5 6 7 8 ETAN ATYP FF0 F 0 6 F 0 7 F 0 8 Variable EPS1 EPS2 EPS3 EPS4 EPS5 EPS6 EPS7 EPS8 Type Default F 0 F 0 F 0 F 0 F 0 F 0 F 0 F Card 4 1 2 3 4 5 6 7 8 Variable ES1 ES2 ES3 ES4 ES5 ES6 ES7 ES8 Type Default Card 5 Variable Type Default F 0 1 L1 F 0 Card 6 1 F 0 2 L2 F 0 2 F 0 3 L3 F 0 3 F 0 4 L4 F 0 4 F 0 5 F 0 6 F 0 7 F 0 8 FF1 FF2 FF3 FF4 F 0 5 F 0 6 F 0 7 F 0 8 Variable LCSS LCLF NUMINT LCF0 LCFC LCFN VGTYP DEXP Type Default F 0 F 0 F 1.0 F 0 F 0 F 0 F 0 F 3.0 VARIABLE DESCRIPTION MID RO E PR SIGY N Material identification. A unique number or label not exceeding 8 characters must be specified. Mass density. Young’s modulus. Poisson’s ratio. Yield stress. Exponent for Power law. This value is only used if ATYP = 1 and LCSS = 0. Q1 Q2 FC F0 EN *MAT_GURSON DESCRIPTION Gurson flow function parameter 𝑞1. Gurson flow function parameter 𝑞2. Critical void volume fraction 𝑓𝑐 where voids begin to aggregate. This value is only used if LCFC = 0. Initial void volume fraction 𝑓0. This value is only used if LCF0 = 0. Mean nucleation strain 𝜀𝑁. GT.0.0: Constant value, LT.0.0: Load curve ID = (-EN) which defines mean nucleation strain 𝜀𝑁 as a function of element length. SN Standard deviation 𝑠𝑁 of the normal distribution of 𝜀𝑁. GT.0.0: Constant value, LT.0.0: Load curve ID = (-SN) which defines standard deviation 𝑠𝑁 of the normal distribution of 𝜀𝑁 as a func- tion of element length. FN ETAN Void volume fraction of nucleating particles 𝑓𝑁. This value is only used if LCFN = 0. Hardening modulus. This value is only used if ATYP = 2 and LCSS = 0. ATYP Type of hardening. EQ.0.0: Ideal plastic, EQ.1.0: Power law, 𝜎𝑌 = SIGY. 𝜎𝑌 = SIGY × ( 𝜀𝑝 + SIGY/E SIGY/E 1/N ) EQ.2.0: Linear hardening, 𝜎𝑌 = SIGY + E × ETAN E − ETAN 𝜀𝑝. EQ.3.0: 8 points curve. FF0 Failure void volume fraction 𝑓𝐹. This value is only used if no curve is given by (L1, FF1) – (L4, FF4) and LCFF = 0. EPS1 - EPS8 *MAT_120 DESCRIPTION Effective plastic strain values. The first point must be zero corresponding to the initial yield stress. At least 2 points should be defined. These values are used if ATYP = 3 and LCSS = 0. ES1 - ES8 Corresponding yield stress values to EPS1 – EPS8. These values are used if ATYP = 3 and LCSS = 0. L1 - L4 Element length values. These values are only used if LCFF = 0 FF1 - FF4 LCSS LCFF NUMINT Corresponding failure void volume fraction. These values are only used if LCFF = 0. Load curve ID or Table ID. ATYP is ignored with this option. Load curve ID defining effective stress versus effective plastic strain. Table ID defines for each strain rate value a load curve ID giving the effective stress versus effective plastic strain for that rate . The stress-strain curve for the lowest value of strain rate is used if the strain rate falls below the minimum value. Likewise, the stress-strain curve for the highest value of strain rate is used if the strain rate exceeds the maximum value. NOTE: The strain rate values defined in the table may be given as the natural logarithm of the strain rate. If the first stress-strain curve in the table corresponds to a negative strain rate, LS-DYNA assumes that the natural logarithm of the strain rate value is used. Since the tables are internally discretized to equally space the points, natural logarithms are necessary, for example, if the curves correspond to rates from 10−4 to 104. Load curve ID defining failure void volume fraction 𝑓𝐹 versus element length. Number of integration points which must fail before the element is deleted. This option is available for shells and solids. LT.0.0: |NUMINT| is percentage of integration points/layers which must fail before shell element fails. For fully in- tegrated shells, a methodology is used where a layer fails if one integration point fails and then the given percentage of layers must fail before the element fails. Only available for shells. LCF0 Load curve ID defining initial void volume fraction 𝑓0 versus element length. LCFC LCFN *MAT_GURSON DESCRIPTION Load curve ID defining critical void volume fraction 𝑓𝑐 versus element length. Load curve ID defining void volume fraction of nucleating particles 𝑓𝑁 versus element length. VGTYP Type of void growth behavior. EQ.0.0: Void growth in case of tension and void contraction in case of compression, but never below 𝑓0 (default). EQ.1.0: Void growth only in case of tension. EQ.2.0: Void growth in case of tension and void contraction in case of compression, even below 𝑓0. DEXP Exponent value for damage history variable 16. Remarks: The Gurson flow function is defined as: Φ = 𝜎𝑀 2 + 2𝑞1𝑓 ∗cosh ( 𝜎𝑌 3𝑞2𝜎𝐻 2𝜎𝑌 ) − 1 − (𝑞1𝑓 ∗)2 = 0 where 𝜎𝑀 is the equivalent von Mises stress, 𝜎𝑌 is the yield stress, 𝜎𝐻 is the mean hydrostatic stress. The effective void volume fraction is defined as 𝑓 ∗(𝑓 ) = ⎧𝑓 { ⎨ { ⎩ 𝑓𝑐 + 1/𝑞1 − 𝑓𝑐 𝑓𝐹 − 𝑓𝑐 𝑓 ≤ 𝑓𝑐 (𝑓 − 𝑓𝑐) 𝑓 > 𝑓c The growth of void volume fraction is defined as 𝐺 + 𝑓 ̇ 𝑁 where the growth of existing voids is defined as 𝑓 ̇ = 𝑓 ̇ 𝑝 𝑓 ̇ 𝐺 = (1 − 𝑓 )𝜀̇𝑘𝑘 and nucleation of new voids is defined as 𝑓 ̇ 𝑁 = 𝐴𝜀̇𝑝 with function A 𝐴 = 𝑓𝑁 𝑆𝑁√2𝜋 exp [− ( 𝜀𝑝 − 𝜀𝑁 𝑆𝑁 ) ] Voids are nucleated only in tension. History variables: Shell / Solid Description 1 / 1 4 / 2 5 / 3 6 / 4 7 / 5 Void volume fraction Triaxiality variable σH/σM Effective strain rate Growth of voids Nucleation of voids 11 / 11 Dimensionless material damage value = {⎧ (f−f0) (fc−f0) {⎨ 1 + ⎩ (f−fc) (fF−fc) 𝑓 ≤ 𝑓c 𝑓 > 𝑓c 13 / 13 Deviatoric part of microscopic plastic strain 14 / 14 Volumetric part of macroscopic plastic strain 16 / 16 Dimensionless material damage value = ( 𝑓 −𝑓0 𝑓𝐹−𝑓0 1/DEXP ) *MAT_GURSON_JC This is an enhancement of Material Type 120. This is the Gurson model with additional Johnson-Cook failure criterion (parameters Card 5). This model is available for shell and solid elements. Strain rate dependency can be defined via a table. An extension for void growth under shear-dominated states and for Johnson-Cook damage evolution is optional. Card 1 1 Variable MID 2 RO Type A8 F 3 E F 4 PR F 5 SIGY F 6 N F 7 Q1 F 8 Q2 F Default none none none none none 0.0 none none Card 2 Variable Type Default 1 FC F 0 Card 3 1 2 F0 F 0 2 3 EN F 0 3 4 SN F 0 4 5 FN F 0 5 6 7 8 ETAN ATYP FF0 F 0 6 F 0 7 F 0 8 Variable EPS1 EPS2 EPS3 EPS4 EPS5 EPS6 EPS7 EPS8 Type Default F 0 F 0 F 0 F 0 F 0 F 0 F 0 F Card 4 1 2 3 4 5 6 7 8 Variable SIG1 SIG2 SIG3 SIG4 SIG5 SIG6 SIG7 SIG8 Type Default F 0 Card 5 1 Variable LCDAM Type Default F 0 Card 6 1 F 0 2 L1 F 0 2 F 0 3 L2 F 0 3 F 0 4 D1 F 0 4 F 0 5 D2 F 0 5 F 0 6 D3 F 0 6 F 0 7 D4 F 0 7 F 0 8 LCJC F 0 8 Variable LCSS LCFF NUMINT LCF0 LCFC LCFN VGTYP DEXP Type Default F 0 F 0 F 1 F 0 F 0 F 0 F 0 F 3.0 Optional Card (starting with version 971 release R4) 4 5 6 7 8 Card 7 1 2 Variable KW BETA Type Default F 0 F 0 3 M F 1.0 VARIABLE DESCRIPTION MID RO E PR SIGY N Q1 Q2 FC F0 EN Material identification. A unique number or label not exceeding 8 characters must be specified. Mass density. Young’s modulus. Poisson’s ratio. Yield stress. Exponent for Power law. This value is only used if ATYP = 1 and LCSS = 0. Gurson flow function parameter 𝑞1. Gurson flow function parameter 𝑞2. Critical void volume fraction 𝑓𝑐 where voids begin to aggregate. Initial void volume fraction 𝑓0. This value is only used if LCF0 = 0. Mean nucleation strain 𝜀𝑁. GT.0.0: Constant value, LT.0.0: Load curve ID = (-EN) which defines mean nucleation strain 𝜀𝑁 as a function of element length. SN Standard deviation 𝑠𝑁 of the normal distribution of 𝜀𝑁. GT.0.0: Constant value, LT.0.0: Load curve ID = (-SN) which defines standard deviation 𝑠𝑁 of the normal distribution of 𝜀𝑁 as a func- tion of element length. FN ETAN Void volume fraction of nucleating particles𝑓𝑁. This value is only used if LCFN = 0. Hardening modulus. This value is only used if ATYP = 2 and LCSS = 0. VARIABLE DESCRIPTION ATYP Type of hardening. EQ.0.0: Ideal plastic, EQ.1.0: Power law, 𝜎𝑌 = SIGY. 𝜎𝑌 = SIGY × ( 𝜀𝑝 + SIGY/E SIGY/E 1/N ) EQ.2.0: Linear hardening, 𝜎𝑌 = SIGY + E × ETAN E − ETAN 𝜀𝑝. EQ.3.0: 8 points curve. FF0 Failure void volume fraction 𝑓𝐹. This value is only used if LCFF = 0. EPS1 - EPS8 Effective plastic strain values. The first point must be zero corresponding to the initial yield stress. At least 2 points should be defined. These values are used if ATYP = 3 and LCSS = 0. ES1 - ES8 LCDAM L1 L2 Corresponding yield stress values to EPS1 – EPS8. These values are used if ATYP = 3 and LCSS = 0. Load curve defining scaling factor Λ versus element length. Scales the Johnson-Cook failure strain . If LCDAM = 0, no scaling is performed. Lower triaxiality factor defining failure evolution (Johnson-Cook). Upper triaxiality factor defining failure evolution (Johnson-Cook). D1 - D4 Johnson-Cook damage parameters. LCJC Load curve defining scaling factor for Johnson-Cook failure versus triaxiality . If LCJC > 0, parameters D1, D2 and D3 are ignored. VARIABLE LCSS LCFF NUMINT LCF0 LCFC LCFN DESCRIPTION Load curve ID or Table ID. ATYP is ignored with this option. Load curve ID defining effective stress versus effective plastic strain. Table ID defines for each strain rate value a load curve ID giving the effective stress versus effective plastic strain for that rate . The stress-strain curve for the lowest value of strain rate is used if the strain rate falls below the minimum value. Likewise, the stress-strain curve for the highest value of strain rate is used if the strain rate exceeds the maximum value. NOTE: The strain rate values defined in the table may be given as the natural logarithm of the strain rate. If the first stress-strain curve in the table corresponds to a negative strain rate, LS-DYNA assumes that the natural logarithm of the strain rate value is used. Since the tables are internally discretized to equally space the points, natural logarithms are necessary, for example, if the curves correspond to rates from 10−4 to 104. Load curve ID defining failure void volume fraction 𝑓𝐹 versus element length. Number of through thickness integration points which must fail before the element is deleted. This option is available for shells and solids. LT.0.0: |NUMINT| is percentage of integration points/layers which must fail before shell element fails. For fully in- tegrated shells, a methodology is used where a layer fails if one integration point fails and then the given percentage of layers must fail before the element fails. Only available for shells. Load curve ID defining initial void volume fraction 𝑓0 versus element length. Load curve ID defining critical void volume fraction 𝑓𝑐 versus element length. Load curve ID defining void volume fraction of nucleating particles 𝑓𝑁 versus element length. VARIABLE DESCRIPTION VGTYP Type of void growth behavior. EQ.0.0: Void growth in case of tension and void contraction in case of compression, but never below 𝑓0 (default). EQ.1.0: Void growth only in case of tension. EQ.2.0: Void growth in case of tension and void contraction in case of compression, even below 𝑓0. DEXP Exponent value for damage history variable 16. KW Parameter kω for void growth in shear-dominated states. See remarks. BETA Parameter β in Lode cosine function. See remarks. M Parameter for generalization of Johnson-Cook damage evolution. See remarks. Remarks: The Gurson flow function is defined as: Φ = 𝜎𝑀 2 + 2𝑞1𝑓 ∗cosh ( 𝜎𝑌 3𝑞2𝜎𝐻 2𝜎𝑌 ) − 1 − (𝑞1𝑓 ∗)2 = 0 where 𝜎𝑀 is the equivalent von Mises stress, 𝜎𝑌 is the yield stress, 𝜎𝐻 is the mean hydrostatic stress. The effective void volume fraction is defined as 𝑓 ∗(𝑓 ) = ⎧𝑓 { ⎨ { ⎩ 𝑓𝑐 + 1/𝑞1 − 𝑓𝑐 𝑓𝐹 − 𝑓𝑐 𝑓 ≤ 𝑓𝑐 (𝑓 − 𝑓𝑐) 𝑓 > 𝑓c The growth of void volume fraction is defined as 𝐺 + 𝑓 ̇ 𝑁 where the growth of existing voids is defined as 𝑓 ̇ = 𝑓 ̇ 𝑓 ̇ 𝐺 = (1 − 𝑓 )𝜀̇𝑘𝑘 𝑝 + 𝑘𝜔𝜔(σ)𝑓 (1 − 𝑓 )𝜀̇𝑀 𝑝𝑙 𝜎𝑌 𝜎𝑀 The second term is an optional extension for shear failure proposed by Nahshon and Hutchinson [2008] with new parameter 𝑘𝜔 (=0 by default), effective plastic strain rate in the matrix 𝜀̇𝑀 𝑝𝑙 , and Lode cosin function 𝜔(σ): 𝜔(σ) = 1 − 𝜉 2 − 𝛽 ⋅ 𝜉 (1 − 𝜉 ), 𝜉 = cos(3𝜃) = 27 𝐽3 3 𝜎𝑀 with parameter 𝛽, Lode angle 𝜃 and third deviatoric stress invariant 𝐽3. Nucleation of new voids is defined as 𝑝𝑙 𝑓 ̇ 𝑁 = 𝐴𝜀̇𝑀 with function A 𝐴 = 𝑓𝑁 𝑆𝑁√2𝜋 exp ⎜⎜⎛𝜀𝑀 2 ⎝ 𝑝𝑙 − 𝜀𝑁 ⎟⎟⎞ 𝑆𝑁 ⎠ ⎡ − ⎢⎢ ⎣ ⎤ ⎥⎥ ⎦ Voids are nucleated only in tension. The Johnson-Cook failure criterion is added in this material model. Based on the triaxiality ratio 𝜎𝐻/𝜎𝑀 failure is calculated as: 𝜎𝐻/𝜎𝑀 > 𝐿1 : Gurson model 𝐿1 ≥ 𝜎𝐻/𝜎𝑀 ≥ 𝐿2 : Gurson model and Johnson-Cook failure criteria 𝐿2 < 𝜎𝐻/𝜎𝑀 : Gurson model Johnson-Cook failure strain is defined as 𝜀𝑓 = [𝐷1 + 𝐷2exp (𝐷3 𝜎𝐻 𝜎𝑀 )] (1 + 𝐷4ln 𝜀̇)Λ where 𝐷1, 𝐷2, 𝐷3 and 𝐷4 are the Johnson-Cook failure parameters and Λ is a function for including mesh-size dependency. An alternative expression can be used, where the first term of the above equation (including D1, D2 and D3) is replaced by a general function LCJC which depends on triaxiality 𝜎𝐻 𝜎𝑀 ) (1 + 𝐷4ln𝜀̇)Λ 𝜀𝑓 = LCJC × ( The Johnson-Cook damage parameter 𝐷𝑓 is calculated with the following evolution equation: 𝐷̇ 𝑓 = 𝜀̇𝑝𝑙 𝜀𝑓 ⇒ 𝐷𝑓 = ∑ Δ𝜀𝑝𝑙 𝜀𝑓 . where 𝛥𝜀𝑝𝑙 is the increment in effective plastic strain. The material fails when 𝐷𝑓 reaches 1.0. A more general (non-linear) damage evolution is possible if 𝑀 > 1 is chosen: 𝐷̇ 𝑓 = (1− 1 𝐷𝑓 ) 𝜀̇𝑝𝑙, 𝜀𝑓 𝑀 ≥ 1.0 Shell / Solid Description *MAT_120_JC 1 / 1 4 / 2 5 / 3 6 / 4 7 / 5 8 / 6 9 / 7 0 / 8 Void volume fraction Triaxiality variable σH/σM Effective strain rate Growth of voids Nucleation of voids Johnson-Cook failure strain εf Johnson-Cook damage parameter Df Domain variable: EQ.0 elastic stress update EQ.1 region (a) Gurson EQ.2 region (b) Gurson + Johnson-Cook EQ.3 region (c) Gurson 11 / 11 Dimensionless material damage value = {⎧ (f−f0) (fc−f0) {⎨ 1 + ⎩ (f−fc) (fF−fc) 𝑓 ≤ 𝑓c 𝑓 > 𝑓c 13 / 13 Deviatoric part of microscopic plastic strain 14 / 14 Volumetric part of macroscopic plastic strain 16 / 16 Dimensionless material damage value = ( 1/DEXP f−f0 fF−f0 ) *MAT_GURSON_RCDC This is an enhancement of material Type 120. This is the Gurson model with the Wilkins Rc-Dc [Wilkins, et al., 1977] fracture model added. This model is available for shell and solid elements. A detailed description of this model can be found in the following references: Gurson [1975, 1977]; Chu and Needleman [1980]; and Tvergaard and Needleman [1984]. Card 1 1 Variable MID 2 RO Type A8 F 3 E F 4 PR F 5 SIGY F 6 N F 7 Q1 F 8 Q2 F Default none none none none none 0.0 none none Card 2 Variable Type Default 1 FC F 0 Card 3 1 2 F0 F 0 2 3 EN F 0 3 4 SN F 0 4 5 FN F 0 5 6 7 8 ETAN ATYP FF0 F 0 6 F 0 7 F 0 8 Variable EPS1 EPS2 EPS3 EPS4 EPS5 EPS6 EPS7 EPS8 Type Default F 0 F 0 F 0 F 0 F 0 F 0 F 0 F Card 4 1 2 3 4 5 6 7 8 Variable ES1 ES2 ES3 ES4 ES5 ES6 ES7 ES8 Type Default Card 5 Variable Type Default F 0 1 L1 F 0 Card 6 1 F 0 2 L2 F 0 2 F 0 3 L3 F 0 3 Variable LCSS LCLF NUMINT Type Default F 0 Card 7 1 F 0 2 F 1 3 F 0 4 L4 F 0 4 4 Variable ALPHA BETA GAMMA D0 Type Default F 0 F 0 F 0 F 0 F 0 5 F 0 6 F 0 7 F 0 8 FF1 FF2 FF3 FF4 F 0 5 5 B F 0 F 0 6 F 0 7 6 7 LAMBDA DS F 0 F 0 F 0 8 8 L F VARIABLE DESCRIPTION MID RO E PR SIGY N Q1 Q1 FC F0 EN SN FN Material identification. A unique number or label not exceeding 8 characters must be specified. Mass density. Young’s modulus. Poisson’s ratio. Yield stress. Exponent for Power law. This value is only used if ATYP = 1 and LCSS = 0. Parameter 𝑞1. Parameter 𝑞2. Critical void volume fraction 𝑓𝑐 Initial void volume fraction 𝑓0. Mean nucleation strain𝜀𝑁. Standard deviation 𝑆𝑁 of the normal distribution of 𝜀𝑁. Void volume fraction of nucleating particles. ETAN Hardening modulus. This value is only used if ATYP = 2 and LCSS = 0. ATYP Type of hardening. EQ.0.0: Ideal plastic, EQ.1.0: Power law, 𝜎𝑌 = SIGY. 𝜎𝑌 = SIGY × ( 𝜀𝑝 + SIGY/E SIGY/E 1/N ) EQ.2.0: Linear hardening, 𝜎𝑌 = SIGY + E × ETAN E − ETAN 𝜀𝑝. EQ.3.0: 8 points curve. FF0 Failure void volume fraction. This value is used if no curve is given by the points (L1, FF1) – (L4, FF4) and LCLF = 0. VARIABLE EPS1 - EPS8 DESCRIPTION Effective plastic strain values. The first point must be zero corresponding to the initial yield stress. This option is only used if ATYP equal to 3. At least 2 points should be defined. These values are used if ATYP = 3 and LCSS = 0. ES1 - ES8 Corresponding yield stress values to EPS1 - EPS8. These values are used if ATYP = 3 and LCSS = 0. L1 - L4 Element length values. These values are only used if LCLF = 0. FF1 - FF4 Corresponding failure void volume fraction. These values are only used if LCLF = 0. LCSS LCLF Load curve ID defining effective stress versus effective plastic strain. ATYP is ignored with this option. Load curve ID defining failure void volume fraction versus element length. The values L1 - L4 and FF1 - FF4 are ignored with this option. NUMINT Number of through thickness integration points which must fail before the element is deleted. ALPHA Parameter 𝛼. for the Rc-Dc model BETA Parameter𝛽. for the Rc-Dc model GAMMA Parameter 𝛾. for the Rc-Dc model D0 B Parameter 𝐷0. for the Rc-Dc model Parameter 𝑏. for the Rc-Dc model LAMBDA Parameter 𝜆. for the Rc-Dc model Parameter 𝐷𝑠. for the Rc-Dc model Characteristic element length for this material DS L Remarks: The Gurson flow function is defined as: Φ = 𝜎𝑀 2 + 2𝑞1𝑓 ∗cosh ( 𝜎𝑌 3𝑞2𝜎𝐻 2𝜎𝑌 ) − 1 − (𝑞1𝑓 ∗)2 = 0 where 𝜎𝑀 is the equivalent von Mises stress, 𝜎𝑌 is the Yield stress, 𝜎𝐻 is the mean hydrostatic stress. The effective void volume fraction is defined as 𝑓 ∗(𝑓 ) = ⎧𝑓 { ⎨ { ⎩ 𝑓𝑐 + 1/𝑞1 − 𝑓𝑐 𝑓𝐹 − 𝑓𝑐 𝑓 ≤ 𝑓𝑐 (𝑓 − 𝑓𝑐) 𝑓 > 𝑓c The growth of the void volume fraction is defined as where the growth of existing voids is given as: 𝑓 ̇ = 𝑓 ̇ 𝐺 + 𝑓 ̇ 𝑁 and nucleation of new voids as: in which 𝐴 is defined as 𝑝 , 𝑓 ̇ 𝐺 = (1 − 𝑓 )𝜀̇𝑘𝑘 𝑓 ̇ 𝑁 = 𝐴𝜀̇𝑝 𝐴 = 𝑓𝑁 𝑆𝑁√2𝜋 exp (− ( 𝜀𝑝 − 𝜀𝑁 𝑆𝑁 ) ) The Rc-Dc model is defined as the following: The damage 𝐷 is given by where 𝜀𝑝 is the equivalent plastic strain, 𝐷 = ∫ 𝜔1𝜔2𝑑𝜀𝑝 𝜔1 = ( 1 − 𝛾𝜎𝑚 ) is a triaxial stress weighting term and 𝜔2 = (2 − 𝐴𝐷)𝛽 is a asymmetric strain weighting term. In the above 𝜎𝑚 is the mean stress and 𝐴𝐷 = max ( 𝑆2 𝑆3 , 𝑆2 𝑆1 ) Fracture is initiated when the accumulation of damage is 𝐷𝑐 > 1 where 𝐷𝑐 is the a critical damage given by 𝐷𝑐 = 𝐷0(1 + 𝑏|∇𝐷|𝜆) *MAT_120_RCDC 𝐹 = 𝐷 − 𝐷𝑐 𝐷𝑠 defines the degradations of the material by the Rc-Dc model. The characteristic element length is used in the calculation of ∇𝐷. Calculation of this factor is only done for element with smaller element length than this value. *MAT_GENERAL_NONLINEAR_1DOF_DISCRETE_BEAM This is Material Type 121. This is a very general spring and damper model. This beam is based on the MAT_SPRING_GENERAL_NONLINEAR option and is a one- dimensional version of the 6DOF_DISCRETE_BEAM above. The forces generated by this model act along a line between the two connected nodal points. Additional unloading options have been included. Card 1 1 Variable MID Type A8 Card 2 1 2 RO F 2 3 K F 3 4 5 6 7 8 IUNLD OFFSET DAMPF I 4 F 5 F 6 7 8 Variable LCIDT LCIDTU LCIDTD LCIDTE Type I Card 3 1 I 2 Variable UTFAIL UCFAIL Type F F I 3 IU F I 4 5 6 7 8 VARIABLE DESCRIPTION MID RO K Material identification. A unique number or label not exceeding 8 characters must be specified. Mass density, see also volume in *SECTION_BEAM definition. Translational stiffness for unloading option 2.0. VARIABLE DESCRIPTION IUNLD Unloading option (Also see Figure M119-1): EQ.0.0: Loading and unloading follow loading curve EQ.1.0: Loading follows loading curve, unloading follows unloading curve. The unloading curve ID if undefined is taken as the loading curve. EQ.2.0: Loading follows loading curve, unloading follows unloading stiffness, K, to the unloading curve. The loading and unloading curves may only intersect at the origin of the axes. EQ.3.0: Quadratic unloading from peak displacement value to a permanent offset. Offset to determine permanent set upon unloading if the IUNLD = 3.0. The permanent sets in compression and tension are equal to the product of this offset value and the maximum compressive and tensile displacements, respectively. Damping factor for stability. Values in the neighborhood of unity are recommended. This damping factor is properly scaled to eliminate time step size dependency. Also, it is active if and only if the local stiffness is defined. Load curve ID defining translational force resultant along the axis versus relative translational displacement. If zero, no stiffness related forces are generated for this degree of freedom. The loading curves must be defined from the most negative displacement to the most positive displacement. The force does not need to increase monotonically for the loading curve. The curves are extrapolated when the displacement range falls outside the curve definition. Load curve ID defining translational force resultant along the axis versus relative translational displacement during unloading. The force values defined by this curve must increase monotonically from the most negative displacement to the most positive displacement. For IUNLD = 1.0, the slope of this curve must equal or exceed the loading curve for stability reasons. This is not the case for IUNLD = 2.0. For loading and unloading to follow the same path simply set LCIDTU = LCIDT. OFFSET DAMPF LCIDT LCIDTU LCIDTD Load curve ID defining translational damping force resultant along the axis versus relative translational velocity. LCIDTE UTFAIL UCFAIL *MAT_GENERAL_NONLINEAR_1DOF_DISCRETE_BEAM DESCRIPTION Load curve ID defining translational damping force scale factor versus relative displacement along the axis. Optional, translational displacement at failure in tension. If zero, failure in tension is not considered. Optional, translational displacement at failure in compression. If zero, failure in compression is not considered. IU Initial translational displacement along axis. *MAT_122 This is Material Type 122. This is Hill’s 1948 planar anisotropic material model with 3 R values. Card 1 1 Variable MID Type A8 Card 2 1 2 RO F 2 3 E F 3 4 PR F 4 Variable R00 R45 R90 LCID F 2 F 3 Type F Card 3 1 Variable AOPT Type F Card 4 1 2 3 Variable Type Card 5 Variable 1 V1 Type F 2 V2 F 3 V3 F F 4 4 A1 F 4 D1 F 5 HR F 5 E0 F 5 5 A2 F 5 D2 F 6 P1 F 6 7 P2 F 7 8 8 6 7 8 6 A3 F 6 D3 F 7 8 7 8 BETA MID RO E PR HR *MAT_HILL_3R DESCRIPTION Material identification. A unique number or label not exceeding 8 characters must be specified. Mass density. Young’s modulus, E Poisson’s ratio, ν Hardening rule: EQ.1.0: linear (default), EQ.2.0: exponential. EQ.3.0: load curve P1 Material parameter: HR.EQ.1.0: Tangent modulus, HR.EQ.2.0: k, strength coefficient for exponential hardening P2 Material parameter: HR.EQ.1.0: Yield stress HR.EQ.2.0: n, exponent R00 R45 R90 R00, Lankford parameter determined from experiments R45, Lankford parameter determined from experiments R90, Lankford parameter determined from experiments LCID load curve ID for the load curve hardening rule E0 𝜀0 for determining initial yield stress for exponential hardening. (Default = 0.0) AOPT *MAT_122 DESCRIPTION Material axes option : EQ.0.0: locally orthotropic with material axes determined by element nodes 1, 2, and 4, as with *DEFINE_COORDI- NATE_NODES, and then rotated about the shell ele- ment normal by an angle BETA. EQ.2.0: globally orthotropic with material axes determined by the vector a defined below, as with *DEFINE_COOR- DINATE_VECTOR. EQ.3.0: locally orthotropic material axes determined by rotating the material axes about the element normal by an angle, BETA, from a line in the plane of the element defined by the cross product of the vector v with the element normal. LT.0.0: the absolute value of AOPT is a coordinate system ID number (CID on *DEFINE_COORDINATE_NODES, *DEFINE_COORDINATE_SYSTEM or *DEFINE_CO- ORDINATE_VECTOR). Available in R3 version of 971 and later. XP YP ZP Coordinates of point p for AOPT = 1. A1 A2 A3 Components of vector a for AOPT = 2. V1 V2 V3 Components of vector v for AOPT = 3. D1 D2 D3 Components of vector d for AOPT = 2. BETA Μaterial angle in degrees for AOPT = 0 and 3, may be overridden on the element card, see *ELEMENT_SHELL_BETA. Remarks: The calculated effective stress is stored in history variable #4. *MAT_HILL_3R_3D This is Material Type 122_3D. It combines orthotropic elastic behavior with Hill’s 1948 anisotropic plasticity theory. Anisotropic plastic properties are given by 6 material parameters, 𝐹, 𝐺, 𝐻, 𝐿, 𝑀, 𝑁 which are determined by experiments. This model is implemented for solid elements. This keyword can be written either as *MAT_HILL_3R_3D, or *MAT_122_3D. Card 1 1 Variable MID Type I Card 2 1 2 RO F 2 3 EX F 3 Variable GXY GYZ GXZ Type F F F 2 HR I 2 3 P1 I/F 3 Card 3 Variable Type 1 N F Card 4 1 Variable AOPT Type I 4 EY F 4 F F 4 P2 F 4 5 EZ F 5 G F 5 6 7 8 PRXY PRYZ PRXZ F 6 H F 6 F 7 L F 7 F 8 M F 8 5 6 7 Card 5 Variable 1 XP Type F Card 6 Variable 1 V1 Type F 2 YP F 2 V2 F 3 ZP F 3 V3 F 4 A1 F 4 D1 F 5 A2 F 5 D2 F 6 A3 F 6 D3 F 7 8 7 8 BETA F VARIABLE DESCRIPTION MID RO EX, EY, EZ Material identification ID, must be a unique number. Mass density. Young’s modulus in 𝑥, 𝑦, and 𝑧 directions, respectively. Negative values indicate (positive) curve numbers, where each curve is a function of temperature. PRXY, PRYZ, PRXZ Poisson’s ratio, 𝜈, in 𝑥𝑦, 𝑦𝑧 and 𝑥𝑧 directions, respectively. Negative values indicate (positive) curve numbers, where each curve is a function of temperature. GXY, GYZ, GXZ F, G, H, L, M, N Shear modulus in 𝑥𝑦, 𝑦𝑧 and 𝑥𝑧 directions, respectively. Negative values indicate (positive) curve numbers, where each curve is a function of temperature. Material constants in Hill’s 1948 yield criterion . Negative values indicate (positive) curve numbers, where each curve is a function of temperature. HR Hardening rule: EQ.1: Stress-strain relationship is defined by load curve or 2D-table ID with parameter P1. P2 is ignored. EQ.2: Stress-strain relationship is defined by strength coefficient K (P1) and strain hardening coefficient n (P2), as in Swift’s exponential hardening equa- tion: 𝜎yield = 𝑘(𝜀 + 0.01)𝑛. VARIABLE DESCRIPTION P1 Material parameter: HR.EQ.1: Load curve or 2D-table ID defining stress- strain curve. If 2D-table ID, the table gives stress-strain curves for different temperatures. HR.EQ.2: 𝑘, strength coefficient in 𝜎yield = 𝑘(𝜀 + 0.01)𝑛. P2 Material parameter: HR.EQ.1: not used. HR.EQ.2.0: 𝑛, the exponent in 𝜎𝑦𝑖𝑒𝑙𝑑 = 𝑘(𝜀 + 0.01)𝑛. AOPT Material axes option : EQ.0.0: locally orthotropic with material axes determined by element nodes 1, 2, and 4, as with *DEFINE_COORDINATE_NODES. EQ.1.0: locally orthotropic with material axes determined by a point 𝐩 in space and the global location of the element center; this is the a- direction. This option is for solid elements only. EQ.2.0: globally orthotropic with material axes determined by the vectors 𝐚 and 𝐝, as with *DE- FINE_COORDINATE_VECTOR. EQ.3.0: locally orthotropic material axes determined by rotating the material axes about the element normal by an angle, BETA, from a line in the plane of the element defined by the cross prod- uct of the vector 𝐯 with the element normal. LT.0.0: the absolute value of AOPT is a coordinate system ID number (CID on *DEFINE_COORDI- NATE_NODES, *DEFINE_COORDINATE_SYS- TEM or *DEFINE_COORDINATE_VECTOR). XP, YP, ZP Coordinates of point 𝐩 for AOPT = 1. A1, A2, A3 Components of vector 𝐚 for AOPT = 2. V1, V2, V3 Components of vector 𝐯 for AOPT = 3. D1, D2, D3 Components of vector 𝐝 for AOPT = 2. BETA *MAT_122_3D DESCRIPTION Material angle in degrees for AOPT = 3, may be overridden on the element card, see *ELEMENT_SHELL_BETA or *EL- EMENT_SOLID_ORTHO. Hill’s 1948 yield criterion: Hill’s yield criterion is based on the assumptions that the material is orthotropic, that hydrostatic stress does not affect yielding, and that there is no Bauschinger effect. According to Hill, when the principal axes of anisotropy are the axes of reference, the yield surface has the form where the effective stress 𝜎̅̅̅̅̅ (stored as history variable #2) is given by 𝑓 = 𝜎̅̅̅̅̅(𝝈) − 𝜎yield(𝜀𝑝) = 0, (𝐹 + 𝐺)𝜎̅̅̅̅̅ 2 = 𝐹(𝜎𝑦 − 𝜎𝑧) + 𝐺(𝜎𝑧 − 𝜎𝑥)2 + 𝐻(𝜎𝑥 − 𝜎𝑦) + 2𝐿𝜏𝑦𝑧 2 + 2𝑀𝜏𝑧𝑥 2 , 2 + 2𝑁𝜏𝑥𝑦 and where 𝐹, 𝐺, 𝐻, 𝐿, 𝑀, 𝑁 are material parameters of the current state of anisotropy, assuming three mutually orthogonal planes of symmetry at every point. The material 𝑧- direction is here the reference direction. Let 𝑋, 𝑌, 𝑍 be the tensile yield stresses in the principal directions of anisotropy, then 𝜎y0 𝑋2 = 𝐺 + 𝐻 𝐹 + 𝐺 , 𝜎y0 𝑌2 = 𝐻 + 𝐹 𝐹 + 𝐺 , 𝜎y0 𝑍2 = 1, where 𝜎y0 = 𝜎yield(0). 𝐹, 𝐺, 𝐻 are not uniquely determined, but the choice F+G = 1 gives 𝐹 = 𝑍2 ( 𝑌2 + 𝑍2 − 𝑋2) , 𝐺 = 𝑍2 𝑋2 + ( 𝑍2 − 𝑌2) , 𝐻 = 𝑍2 ( 𝑋2 + 𝑌2 − 𝑍2). Material F G H L M N AA5042 0.3341 0.5098 0.3569 1.5000 1.5000 1.8197 Table M122-1. NUMISHEET 2011. AA5042 material constants (Hill’s 1948 yield) - BM1 If 𝑅𝑥𝑦 , 𝑆𝑧𝑥 , 𝑇𝑥𝑦 are the yield stresses in shear with respect to the principal axes of anisotropy, then 𝐿 = 𝑍2 2 , 2𝑅𝑥𝑦 𝑀 = 𝑍2 2 , 2𝑆𝑧𝑥 𝑁 = 𝑍2 2 . 2𝑇𝑥𝑦 If 𝐹 = 𝐺 = 𝐻, and, 𝐿 = 𝑀 = 𝑁 = 3𝐹, the Hill criterion reduces to the Von-Mises criterion. The strain hardening in this model can either defined by the load curve or by Swift’s exponential hardening equation: 𝜎yield = 𝑘(𝜀 + 0.01)𝑛. Validation and application: 1. This material model is suitable for metal forming application using solid elements to account for anisotropic plasticity. NUMISHEET conferences have provided material constants of Hill’s 1948 yield for many commonly used ma- terials. In this example, experimental results from benchmark 1 (BM1, AA5042) of the NUMISHEET 2011 are used to validate an equal-biaxial tension and two uniaxial tensile results in two different directions (rolling and 90°) on a single solid element. As shown in Figure M122-1(top left), under the constraints imposed, a single element of solid type 2 is pulled in uniaxial tension in the 𝑥-direction. The resulting hardening curve is compared with experimental data provided (top right). Similarly, the element is pulled in uniaxial tension in the Y-direction under the constraints shown in Figure M122-1(middle left). The resulting hard- ening curve is compared with experimental data (middle right). In Figure M122-1(bottom left), the element is pulled in both 𝑥- and 𝑦-directions equally under the constraints shown, and the resulting hardening curve is compared with experimental data (bottom right). All computed results are satisfactory. The material constants used for the simulation are provided in Table M122-1. In addition, an element of type 1 is subjected to a shear test with a composite material, courtesy of CYBERNET SYSTEMS CO., LTD. Results compare well with the experiments, as shown in Figure M122-2. In real world application, the six material parameters required can be calibrated with nonlinear regression analysis (such as those available through LS-OPT) through a series of tensile tests in three orthogonal directions and three shear tests in three orthogonal planes. 2. This material model can also be applied in multi-scale simulation of fiberglass and laminated materials, according to CYBERNET SYSTEMS CO., LTD. The elastic coefficients can be calibrated analytically by a homogenization method with tensile tests in the three orthogonal directions and three pure shear tests in the three orthogonal planes. Revision information: The material model is available in explicit dynamics in both SMP and MPP starting in Revision 86100, and is available in implicit dynamics in both SMP and MPP starting in Revision 104178. It also supports temperature dependent Young’s/shear modulus, Poisson ratios, and Hill parameters. 0= *MAT_HILL_3R_3D Rolling direction (0 deg.) tensile pull ux Fy 0= ) ( 500.0 400.0 300.0 200.0 100.0 0.0 ) ( 500.0 400.0 300.0 200.0 100.0 0.0 ) ( 500.0 400.0 300.0 200.0 100.0 0.0 Fz 0= Fz 0= uy ux uy Experiment LS-DYNA 0.0 0.03 0.08 0.13 0.18 True strain 90 deg. tensile pull Experiment LS-DYNA 0.0 0.03 0.08 0.13 0.18 True strain Equi-biaxial test Experiment LS-DYNA 0.0 0.03 0.08 0.13 0.18 True strain Fy 0= Figure M122-1. Validation with experiments - BM1 NUMISHEET 2011 ux 35.0 30.0 25.0 20.0 10.0 ) ( 0.0 0.0 XY shear test Experiment LS-DYNA 0.01 0.02 0.03 True strain Figure M122-2. Shear result validated with test results (Courtesy of CYBERNET SYSTEMS CO., LTD.) *MAT_MODIFIED_PIECEWISE_LINEAR_PLASTICITY_{OPTION} This is Material Type 123, which is an elasto-plastic material supporting an arbitrary stress versus strain curve as well as arbitrary strain rate dependency. This model is available for shell and solid elements. Another model, MAT_PIECEWISE_LINEAR_ PLASTICITY, is similar but lacks the enhanced failure criteria. Failure is based on effective plastic strain, plastic thinning, the major principal in plane strain component, or a minimum time step size. See the discussion under the model description for MAT_ PIECEWISE_LINEAR_PLASTICITY if more information is desired. Available options include: <BLANK> RATE RTCL STOCHASTIC (for shells only) The “RATE” option is used to account for rate dependence of plastic thinning failure. The “RTCL” option is used to activate RTCL damage. One additional card is needed with either option. Card 1 1 Variable MID 2 RO Type A8 F 3 E F 4 PR F 5 6 7 8 SIGY ETAN FAIL TDEL F F F Default none none none none none 0.0 10.E+20 Card 2 Variable Type Default 1 C F 0 2 P F 0 3 4 5 6 7 LCSS LCSR VP EPSTHIN EPSMAJ NUMINT F 0 F 0 F 0 F 0 F 0 F 0 F 0 Card 3 1 2 3 4 5 6 7 8 Variable EPS1 EPS2 EPS3 EPS4 EPS5 EPS6 EPS7 EPS8 Type Default F 0 Card 4 1 F 0 2 F 0 3 F 0 4 F 0 5 F 0 6 F 0 7 F 0 8 Variable ES1 ES2 ES3 ES4 ES5 ES6 ES7 ES8 Type Default F 0 F 0 F 0 F 0 F 0 F 0 F 0 F 0 Card 5 is required if and only if either the RATE or RTCL option is active. Card 5 1 2 3 4 5 6 7 8 Variable LCTSRF EPS0 TRIAX Type Default I 0 F 0 F 0 VARIABLE DESCRIPTION MID RO E PR Material identification. A unique number or label not exceeding 8 characters must be specified. Mass density. Young’s modulus. Poisson’s ratio. SIGY Yield stress. *MAT_MODIFIED_PIECEWISE_LINEAR_PLASTICITY DESCRIPTION ETAN Tangent modulus, ignored if (LCSS.GT.0) is defined. FAIL Failure flag. LT.0.0: User defined failure subroutine, matusr_24 in dyn21.F, is called to determine failure EQ.0.0: Failure is not considered. This option is recommended if failure is not of interest since many calculations will be saved. GT.0.0: Plastic strain to failure. When the plastic strain reaches this value, the element is deleted from the calculation. TDEL Minimum time step size for automatic element deletion. C P Strain rate parameter, C, see formula below. Strain rate parameter, P, see formula below. LCSS Load curve ID or Table ID. Load Curve. When LCSS is a Load curve ID, it is taken as defining effective stress versus effective plastic strain. If defined EPS1 - EPS8 and ES1 - ES8 are ignored. Tabular Data. The table ID defines for each strain rate value a load curve ID giving the stress versus effective plastic strain for that rate, See Figure M24-1. When the strain rate falls below the minimum value, the stress versus effective plastic strain curve for the lowest value of strain rate is used. Likewise, when the strain rate exceeds the maximum value the stress versus effective plastic strain curve for the highest value of strain rate is used. The strain rate parameters: C and P, the curve ID, LCSR, EPS1 - EPS8, and ES1 - ES8 are ignored if a Table ID is defined. Logarithmically Defined Tables. If the first stress-strain curve in the table corresponds to a negative strain rate, LS-DYNA assumes that the natural logarithm of the strain rate value is used for all stress-strain curves. Since the tables are internally discretized to equally space the points, natural logarithms are necessary, for example, if the curves correspond to rates from 10−4 to 104. Computing natural logarithms can substantially increase the computational time on certain computer architectures. LCSR Load curve ID defining strain rate scaling effect on yield stress. VARIABLE DESCRIPTION VP Formulation for rate effects: EQ.0.0: Scale yield stress (default), EQ.1.0: Viscoplastic formulation (recommended). EPSTHIN Thinning strain at failure. This number should be given as a positive number. EPSMAJ Major in plane strain at failure. NUMINT EPS1 - EPS8 LT.0: EPSMAJ = |EPSMAJ| and filtering is activated. The last twelve values of the major strain is stored at each integra- tion point and the average value is used to determine failure. Number of integration points which must fail before the element is deleted. (If zero, all points must fail.) For fully integrated shell formulations, each of the 4 × NIP integration points are counted individually in determining a total for failed integration points. NIP is the number of through-thickness integration points. As NUMINT approaches the total number of integration points (NIP for under integrated shells, 4*NIP for fully integrated shells), the chance of instability increases. LT.0.0: |NUMINT| is percentage of integration points/layers which must fail before shell element fails. For fully in- tegrated shells, a methodology is used where a layer fails if one integration point fails and then the given percentage of layers must fail before the element fails. Only available for shells. Effective plastic strain values (optional if SIGY is defined). At least 2 points should be defined. The first point must be zero corresponding to the initial yield stress. WARNING: If the first point is nonzero the yield stress is extrapolated to determine the initial yield. If this option is used SIGY and ETAN are ignored and may be input as zero. ES1 - ES8 Corresponding yield stress values to EPS1 - EPS8. LCTSRF Load curve that defines the thinning strain at failure as a function of the plastic strain rate. *MAT_MODIFIED_PIECEWISE_LINEAR_PLASTICITY DESCRIPTION EPS0 EPS0 parameter for RTCL damage. EQ.0.0: (default) RTCL damage is inactive. GT.0.0: RTCL damage is active TRIAX RTCL damage triaxiality limit. EQ.0.0: (default) No limit. GT.0.0: Damage does not accumulate when triaxiality exceeds TRIAX. Remarks: Optional RTCL damage is used to fail elements when the damage function exceeds 1.0. During each solution cycle, if the plastic strain increment is greater than zero, an increment of RTCL damage is calculated by 𝛥𝑓damage = 𝜀0 𝑓 ( 𝜎𝐻 𝜎̅̅̅̅̅ 𝑑𝜀̅𝑝 ) RTCL where and, 𝑓 ( 𝜎𝐻 𝜎̅̅̅̅̅ ) = RTCL ⎧0 {{ {{{{ {{ ⎨ {{ {{{ {{{ ⎩ 1 + 𝜎𝐻 𝜎̅̅̅̅̅ 𝜎𝐻 𝜎̅̅̅̅̅ √12 − 27( + √12 − 27( 1.65 exp ( 3𝜎𝐻 2𝜎̅̅̅̅̅ ) 𝜎𝐻 𝜎̅̅̅̅̅ 𝜎𝐻 𝜎̅̅̅̅̅ 𝜎𝐻 𝜎̅̅̅̅̅ ≤ − ) ) < 𝜎𝐻 𝜎̅̅̅̅̅ < 𝜎𝐻 𝜎̅̅̅̅̅ ≥ 𝜀0 = uniaxial fracture strain / critical damage value 𝜎𝐻 = hydrostatic stress 𝜎̅̅̅̅̅ = effective stress 𝑑𝜀̅𝑝 = effective plastic strain increment The increments are summed through time and the element is deleted when 𝑓damage ≥ 1.0. For 0.0 < 𝑓damage < 1.0, the element strength will not be degraded. The value of 𝑓damage is stored as history variable #9 and can be fringe plotted from d3plot files if the number of extra history variables requested is ≥ 9 on *DATABASE_EX- TENT_BINARY. The optional TRIAX parameter can be used to prevent excessive RTCL damage growth and element erosion for badly shaped elements that might show unrealistically high values for the triaxiality. The triaxiality, 𝜎𝐻 𝜎̅̅̅̅̅ , is stored as history variable #11. The EPSMAJ parameter is compared to the major principal strain in the following senses: • For shells it is the maximum eigenvalue of the in-plane strain tensor that is incremented by the strain increments. • For solid elements it is calculated as the maximum eigenvalue to the logarithmic strain tensor 𝛆 = ln(𝐅T𝐅), where 𝐅 is the global deformation gradient. In sum, both element types use a natural strain measure for determining failure, the major strain calculated in this way is output as history variable #7. To get an idea about the probability of failure, an indicator 𝐷 is computed internally: 𝐷 = max ( 𝜀̅𝑝 FAIL , −𝜀3 EPSTHIN , 𝜀𝐼 EPSMAJ ) and stored as history variable #10. 𝐷 ranges from 0 (intact) to 1 (failed). 𝜀̅𝑝, −𝜀3, and 𝜀𝐼 are current values of effective plastic strain, thinning strain, and major in plane strain. This instability measure, including the RTCL damage, can also be retrieved from requesting material histories *DEFINE_MATERIAL_HISTORIES Properties Label Attributes Description Instability Plastic Strain Rate - - - - - - - - Failure indicator max(𝐷, 𝑓damage) 𝑝 Effective plastic strain rate 𝜀̇eff For implicit calculations on this material involving severe nonlinear hardening the radial return method may result in inaccurate stress-strain response. Setting IACC = 1 on *CONTROL_ACCURACY activates a fully iterative plasticity algorithm, which will remedy this. This is not to be confused with the MITER flag on *CONTROL_SHELL, which governs the treatment of the plane stress assumption for shell elements. If any failure model is applied with this option, incident failure will initiate damage, and the stress will continuously degrade to zero before erosion for a deformation of 1% plastic strain. So for instance, if the failure strain is FAIL = 0.05, then the element is eroded when 𝜀̅𝑝 = 0.06 and the material goes from intact to completely damaged between 𝜀̅𝑝 = 0.05 and 𝜀̅𝑝 = 0.06. The reason is to enhance implicit performance by maintaining continuity in the internal forces. *MAT_PLASTICITY_COMPRESSION_TENSION This is Material Type 124. An isotropic elastic-plastic material where unique yield stress versus plastic strain curves can be defined for compression and tension. Also, failure can occur based on a plastic strain or a minimum time step size. Rate effects on the yield stress are modeled either by using the Cowper-Symonds strain rate model or by using two load curves that scale the yield stress values in compression and tension, respectively. Material rate effects, which are independent of the plasticity model, are based on a 6-term Prony series Maxwell mode that generates an additional stress tensor. The viscous stress tensor is superimposed on the stress tensor generated by the plasticity. Card 1 1 Variable MID 2 RO Type A8 F 3 E F 4 PR F Default none none none none Card 2 1 2 3 4 5 C F 0 5 6 P F 0 6 Variable LCIDC LCIDT LCSRC LCSRT SRFLAG LCFAIL Type Default Card 3 Variable Type Default I 0 1 PC F 0 I 0 2 PT F 0 I 0 3 I 0 4 F 0 5 I 0 6 PCUTC PCUTT PCUTF F 0 F 0 F 0 7 8 FAIL TDEL F 10.E+20 7 EC F none 7 F 0 8 RPCT F 0 3 4 5 6 7 8 *MAT_124 Card 4 Variable Type 1 K F Viscoelastic Constant Cards. Up to 6 cards may be input. A keyword card (with a “*” in column 1) terminates this input if less than 6 cards are used. Card 5 Variable Type 1 Gi F VARIABLE MID RO E PR C P 2 3 4 5 6 7 8 BETAi F DESCRIPTION Material identification. A unique number or label not exceeding 8 characters must be specified. Mass density. Young’s modulus. Poisson’s ratio. Strain rate parameter, 𝐶, see formula below. Strain rate parameter, 𝑃, see formula below. FAIL Failure flag. LT.0.0: User defined failure subroutine, matusr_24 in dyn21.F, is called to determine failure EQ.0.0: Failure is not considered. This option is recommended if failure is not of interest since many calculations will be saved. GT.0.0: Plastic strain to failure. When the plastic strain reaches this value, the element is deleted from the calculation. TDEL Minimum time step size for automatic deletion of shell elements. VARIABLE LCIDC LCIDT LCSRC LCSRT DESCRIPTION Load curve ID defining effective stress versus effective plastic strain in compression. Enter positive yield stress and plastic strain values when defining this curve. Load curve ID defining effective stress versus effective plastic strain in tension. Enter positive yield stress and plastic strain values when defining this curve. Optional load curve ID defining strain rate scaling factor on yield stress versus strain rate when the material is in compression. Optional load curve ID defining strain rate scaling factor on yield stress versus strain rate when the material is in tension. SRFLAG Formulation for rate effects: EQ.0.0: Total strain rate, EQ.1.0: Deviatoric strain rate. EQ.2.0: Plastic strain rate (viscoplastic). LCFAIL EC RPCT PC PT Load curve ID defining failure strain versus strain rate. See Remarks for additional information. Optional Young’s modulus for compression, > 0. Fraction of PT and PC, used to define mean stress at which Young’s modulus is E and EC, respectively. Young’s modulus is E when mean stress > RPCT × PT, and EC when mean stress < - RPCT × PC. If the mean stress falls between –RPCT × PC and RPCT × PT, a linearly interpolated value is used. Compressive mean stress (pressure) at which the yield stress follows load curve ID, LCIDC. If the pressure falls between PC and PT a weighted average of the two load curves is used. Both PC and PT should be entered as positive values. Tensile mean stress at which the yield stress follows load curve ID, LCIDT. PCUTC *MAT_PLASTICITY_COMPRESSION_TENSION DESCRIPTION Pressure cut-off in compression (PCUTC must be greater than or equal to zero). PCUTC (and PCUTT) apply only to element types that use a 3D stress update, e.g., solids, tshell formulations 3 and 5, and SPH. When the pressure cut-off is reached the deviatoric stress tensor is set to zero and the pressure remains at its compressive value. Like the yield stress, PCUTC is scaled to account for rate effects. PCUTT Pressure cut-off in tension (PCUTT must be less than or equal to zero). When the pressure cut-off is reached the deviatoric stress tensor and tensile pressure is set to zero. Like the yield stress, PCUTT is scaled to account for rate effects. PCUTF Pressure cut-off flag activation. EQ.0.0: Inactive, EQ.1.0: Active. K Gi Optional bulk modulus for the viscoelastic material. If nonzero a Kelvin type behavior will be obtained. Generally, 𝐾 is set to zero. Optional shear relaxation modulus for the ith term BETAi Optional shear decay constant for the ith term Remarks: The stress strain behavior follows a different curve in compression than it does in tension. Tension is determined by the sign of the mean stress where a positive mean stress (i.e., a negative pressure) is indicative of tension. Two curves must be defined giving the yield stress versus effective plastic strain for both the tension and compression regimes. Mean stress is an invariant which can be expressed as (𝜎𝑥 + 𝜎𝑦 + 𝜎𝑧)/3. PC and PT define a range of mean stress values within which interpolation is done between the tensile yield surface and compressive yield surface. PC and PT are not true material properties but are just a numerical convenience so that the transition from one yield surface to the other is not abrupt as the sign of the mean stress changes. Both PC and PT are input as positive values as it is implied that PC is a compressive mean stress value and PT is tensile mean stress value. Strain rate may be accounted for using the Cowper and Symonds model which scales the yield stress with the factor: where 𝜀̇ is the strain rate, 1 + [ 𝑝⁄ 𝜀̇ ] 𝜀̇ = √𝜀̇𝑖𝑗𝜀̇𝑖𝑗. The LCFAIL field is only applicable when at least one of the following four conditions are met: 1. SRFLAG = 2 2. LCSRC is nonzero 3. LCSRT is nonzero 4. Gi, BETAi values are provided. *MAT_KINEMATIC_HARDENING_TRANSVERSELY_ANISOTROPIC_{OPTION} This is Material Type 125. This material model combines Yoshida & Uemori’s non- linear kinematic hardening rule with material type 37. Yoshida & Uemori’s theory uses two surfaces to describe the hardening rule: the yield surface and the bounding surface. In the forming process, the yield surface does not change in size, but its center translates with deformation; the bounding surface changes both in size and location. This model also allows the change of Young’s modulus as a function of effective plastic strain as proposed by Yoshida & Uemori [2002]. This material type is available for shells, thick shells and solid elements. Available options include: <BLANK> NLP The NLP option estimates necking failure using the Formability Index (F.I.), which accounts for the non-linear strain paths seen in metal forming applications . Specify IFLD in card #3 when using this option, also see the example under the remarks. Since the NLP option also works under linear strain path, it is recommended to be used as the default failure criterion in metal forming. The NLP option is also available in *MAT_036, *MAT_037, and *MAT_226. Card 1 1 Variable MID 2 RO Type A8 F 3 E F 4 PR F 5 R F I 6 7 8 HLCID OPT Default none none none none none none Card 2 Variable 1 CB Type F 2 Y F 3 SC1 F 4 K F 5 RSAT F 6 SB F I 0 7 H F 8 SC2 F Default none none none none none none none 0.0 Card 3 Variable 1 EA 2 3 COE IOPT Type F F Default none none I 0 4 C1 F 5 C2 F 6 7 8 IFLD I none none none VARIABLE DESCRIPTION MID RO E PR R HLCID OPT CB Y Material identification. A unique number or label not exceeding 8 characters must be specified. Mass density. Young’s Modulus Poisson’s ratio Anisotropic hardening parameter Load curve ID in keyword *DEFINE_CURVE, where true strain and true stress relationship is characterized. This curve is used in conjunction with variable OPT, and not to be referenced or used in other keywords. The use of this parameter is not recommended. Error calculation flag. When OPT = 2, LS-DYNA will perform error calculation based on the true stress-strain curve from uniaxial tension, specified by HLCID. The corrections will be made to the cyclic load curve, both in the loading and unloading portions. Since, in some cases where loading is more complex, the accumulated plastic strain could be large (say more than 30%), the input uniaxial stress-strain curve must have enough strain range to cover the maximum expected plastic strain. Note this variable must be set to a value of “2” if HLCID is specified and stress-strain curve is used. The default value of “0” is recommended. The uppercase 𝐵 defined in Yoshida & Uemori’s equations. Hardening parameter appearing equations. in Yoshida & Uemori’s *MAT_KINEMATIC_HARDENING_TRANSVERSELY_ANISOTROPIC DESCRIPTION SC1 K RSAT SB H SC2 EA COE The lowercase 𝑐 defined in the following equations, and 𝐶1 as in the remarks section. Hardening parameter appearing equations. in Yoshida & Uemori’s Hardening parameter appearing equations. in Yoshida & Uemori’s The lowercase 𝑏 appearing in Yoshida & Uemori’s equations. Anisotropic parameter stagnation. associated with work-hardening The lowercase 𝑐 defined in the following equations, and 𝐶2 as in the remarks section. If SC2 = 0.0, left blank, or SC2 = SC1, then it turns into the basic model. Variable controlling the change of Young’s modulus, 𝐸𝐴 in the following equations. Variable controlling the change of Young’s modulus, 𝜁 in the following equations. IOPT Modified kinematic hardening rule flag: EQ.0: Original Yoshida & Uemori formulation, EQ.1: Modified formulation. Define C1, C2 below. C1, C2 Constants used to modify R: 𝑅 = RSAT × [(𝐶1 + 𝜀̅𝑝)𝑐2 − 𝐶1 𝑐2] IFLD ID of a load curve defining Forming Limit Diagram (FLD) under linear strain paths. In the load curve, abscissas represent minor strains while ordinates represent major strains. Define only when the option NLP is used. See the example in the remarks section. The Yoshida & Uemori’s kinematic hardening model: According to F. Yoshida and T. Uemori’s paper titled “A model of large-strain cyclic plasticity describing the Bauschinger effect and work hardening stagnation” in 2002 International Journal of Plasticity 18, 661-686, and referring to Figure M125-1, 𝛼∗ = 𝛼 − 𝛽 𝛼∗ = 𝑐 [( ) (𝜎 − 𝛼) − √ 𝛼∗ 𝛼∗] 𝜀̅𝑝 𝑎 = 𝐵 + 𝑅 − 𝑌 The change of size and location for the bounding surface is defined as, referring to Figure M125-2, 𝑅̇ = 𝑘(𝑅sat − 𝑅)𝜀̅ 𝛽′ 𝑏𝐷 − 𝛽′𝜀̅ = 𝑘( ̇𝑝, ̇𝑝) In Yoshida & Uemori’s model, there is work-hardening stagnation in the unloading process, and it is described as, 𝜎bound = 𝐵 + 𝑅 + 𝛽 𝑔𝜎(𝜎 ′, 𝑞′, 𝑟′) = (𝜎 ′ − 𝑞′): (𝜎 ′ − 𝑞′) − 𝑟2 𝑞′ = 𝜇(𝛽′ − 𝑞′) 𝑟 = ℎΓ 3(𝛽′ − 𝑞′): 𝛽′ 2𝑟 Γ = The change in Young’s modulus is defined as a function of effective strain, 𝐸 = 𝐸0 − (𝐸0 − 𝐸𝐴)[1 − exp(−𝜁 𝜀̅𝑝)] Strain hardening saturation: in NUMISHEET 2008 proceedings, 137-142, 2008, Further improvements in the original Yoshida & Uemori’s model, as described in a paper “Determination of Nonlinear Isotropic/Kinematic Hardening Constitutive Parameter for AHSS using Tension and Compression Tests”, by Ming F. Shi, Xinhai Zhu, Cedric Xia, Thomas Stoughton, included modifications to allow working hardening in large strain deformation region, avoiding the problem of earlier saturation, especially for Advanced High Strength Steel (AHSS). These types of steels exhibit continuous strain hardening behavior and a non-saturated isotropic hardening function. As described in the paper, the evolution equation for R (a part of the current radius of the bounding surface in deviatoric stress space), as is with the saturation type of isotropic hardening rule proposed in the original Yoshida & Uemori model, 𝑅̇ = 𝑚(𝑅sat − 𝑅)𝑝̇ is modified as, 𝑅 = RSAT × [(𝐶1 + 𝜀̅𝑝)𝑐2 − 𝐶1 𝑐2] For saturation type of isotropic hardening rule, set IOPT = 0, applicable to most of Aluminum sheet materials. In addition, the paper provides detailed variables used for this material model for DDQ, HSLA, DP600, DP780 and DP980 materials. Since the symbols used in the paper are different from what are used here, the following table provides a reference between symbols used in the paper and variables here in this keyword: B CB Y Y C SC1 m K K Rsat b SB h H e0 C1 N C2 Using the modified formulation and the material properties provided by the paper, the predicted and tested results compared very well both in a full cycle tension and compression test and in a pre-strained tension and compression test, according to the paper. A Failure Criterion for Nonlinear Strain Paths (NLP): The NLP failure criterion and corresponding post processing procedures are described in the entries for *MAT_036 and *MAT_037. The history variables for every element stored in d3plot files include: 1. Formability Index (F.I.): #1 2. Strain ratio (in-plane minor strain/major strain): #2 3. Effective strain from the planar isotropic assumption: #3 The entire time history can be plotted using Post/History menu in LS-PrePost v4.0. To enable the output of these history variables to the d3plot files, NEIPS on the *DATA- BASE_EXTENT_BINARY card must be set to at least 3. When plotting the formability index, first select the history var #1 from the Misc in the FriComp menu. The pull-down menu under FriComp can be used to select minimum value ‘Min’ for necking failure determination (refer to Tharrett and Stoughton’s paper in 2003 SAE 2003-01-1157). In FriRang, the option None is to be selected in the pull-down menu next to Avg. Lastly, set the simulation result to the last state in the animation tool bar. The index value ranges from 0.0 to 1.5. The non-linear forming limit is reached when the index reaches 1.0. An Example of the NLP Option: A partial keyword example is listed below when the option NLP is used. The traditional Forming Limit Diagram (FLD) which governs the linear strain paths only is defined by load curve ID 321. *MAT_KINEMATIC_HARDENING_TRANSVERSELY_ANISOTROPIC_NLP $# mid ro e pr r hclid opt 1 7.83E-9 2.07E+5 0.3 1.035 $# cb y sc k rsat sb h 422.8 304.2 398.5 28.0 702.7 136.9 0.91 $# ea coe iopt c1 c2 IFLD 0.0 0.0 1 0.0065 0.545 321 *DEFINE_CURVE $ traditional FLD data (major vs. minor) 321 -0.357,0.596 ⋮ ⋮ -0.020,0.260 0.000,0.239 0.010,0.244 0.020,0.249 ⋮ ⋮ 0.239,0.354 0.247,0.356 0.262,0.361 0.372,0.361 *END Application results: Application of the modified Yoshida & Uemori’s hardening rule in the metal forming industry has shown significant advantage in springback prediction accuracy, especially for AHSS type of sheet materials. As shown in Figure M125-3 (left), predicted springback shape of an automotive shotgun (also called: upper load path/beam) using *MAT_125 is compared with experimental measurements on a DP780 material. Prediction accuracy achieved over 92% with *MAT_125 while about 61% correlation is found with *MAT_037 (Figure M125-3 right), a remarkable improvement. In another example, NUMISHEET 2011 BM4 is used to demonstrate the application of the Young’s modulus variations as a function of effective strain in prediction of springback. The sheet blank is a DP780 material with an initial thickness of 1.4mm. The simulation process is shown (Figure M125-4) as pre-straining (to 8%), springback, trimming, forming and springback. Young’s modulus variations with effective strains are accounted for by curve fitting the provided experimental data to obtain the variables EA and COE, Figure M125-5. Referring to Figures M125-6 and M125-7, final springback shapes of the cross sectional view are compared with measurement provided, along with benchmark results from software X and Y. In addition, springback with no pre-straining is also conducted and correlated, shown in the same figures. Furthermore, hysteretic plasticity with a full cycle tension and compression simulation is done on one single shell element and the result is superimposed with experimental date, in Figure M125-8. To improve convergence and for a faster simulation time, it is recommended that *CONTROL_IMPLICIT_FORMING type ‘1’ be used when conducting a springback simulation. About SC1 and SC2: In F. Yoshida and T. Uemori’s 2002 paper, the effect of variables SC1 and SC2 were discussed. According to the paper, variables SC1 and SC2 are used to describe the forward and reverse deformations of the cyclic plasticity curve, respectively. It allows for a more rapid change of work hardening rate in the vicinity of the initial yielding (~0.5% equivalent plastic strain), in the form of the following equations: SC = ⎧ {{ ⎨ {{ ⎩ SC1 max(𝛼̅∗) < 𝐵 − 𝑌 SC2 otherwise where max(𝛼̅∗) is the maximum value of 𝛼̅∗, and, 𝛼̅∗ = √ 𝛼∗: 𝛼∗ As shown in Figure M125-9 from Yoshida & Uemori’s original paper, the effect of a curve fitting is shown for a high strength steel (SPFC) using both SC1 and SC2, which fits much better than the fitting using only SC1. In addition, in Figure M125-10, a much better fitting is demonstrated with SC1 and SC2 than with SC1 only for a DP980 material. Inclusion of shell normal stress: When *LOAD_SURFACE_STRESS is used in the input deck together with *MAT_125, normal stresses (either from sliding contact or applied pressure) are accounted for during the simulation. The negative local 𝑧-stresses (select z-stress under FCOMP → Stress and select local under FCOMP in LS-PrePost) caused by the sliding contact or applied pressure can be viewed from d3plot files after Revision 97158. It is found in some cases this inclusion can improve forming simulation accuracy. Revision information: The variables HLCID, OPT, IOPT, C1, and C2 are available starting in Revision 46217. The variables SC1 and SC2 are available starting in Revision 74884. The option NLP is available in explicit dynamic analysis starting in Revision 95594. Normal stresses inclusion is available starting in Revision 97158. Later Revisions include various improvements and should be used. Bounding surface Dp Yield surface * B+R Figure M125-1. Schematic illustration of the two-surface model is the original center of the yield surface, 𝛼∗ is the current center for the yield surface; 𝛼 is the center of the bounding surface. 𝛽 represents the relative position of the centers of the two surfaces. Y is the size of the yield surface and is constant throughout the deformation process. B+R represents the size of the bounding surface, with R being associated with isotropic hardening. Reproduced from the original Yoshida and Uemori’s paper. Bounding surface F β' q' gσ gσ β' q'o β' q' (a) when R = 0 (b) when R > 0 Figure M125-2. Change in bounding surface (reproduced from the original Yoshida and Uemori’s paper). Red: measured Black: simulation 92.51% of sampled points within 1mm deviation 61.78% of sampled points within 1mm deviation Max. 6.63mm Max. 2.42mm *MAT_125 *MAT_037 Figure M125-3. Comparison of springback prediction on the A/S P load beam (reproduced from an original color contour map courtesy of Chrysler LLC and United States Steel Corporation). Blanking Pre-straining Springback Trimming Forming Forming complete Springback Figure M125-4. NUMISHEET 2011 Benchmark #4 simulation procedure. ) ( ' 200 195 190 185 180 175 170 165 Young's Modulus Evolution Fitted for LS-DYNA Test 0.02 0.04 0.06 0.08 0.10 0.12 Equivalent plastic strain Figure M125-5. Curve fitting with coefficients: EA = 1.668E+05; COE = 95.0. Springback Profile: No Prestrain Springback Profile: 8% Prestrain 70 60 50 40 30 20 10 0 Test LS-DYNA Software X 0 20 40 60 80 100 120 140 mm 70 60 50 40 30 20 10 0 Test LS-DYNA Software X 0 20 40 60 mm 80 100 120 Figure M125-6. Comparison of springback profile with software X: 0% (left) and 8% prestrain (right) Springback Profile: No Prestrain Springback Profile: 8% Prestrain 70 60 50 40 30 20 10 0 Test LS-DYNA Software Y 0 20 40 60 80 100 120 140 mm 70 60 50 40 30 20 10 0 Test LS-DYNA Software Y 0 20 40 60 mm 80 100 120 Figure M125-7. Comparison of springback profile with software Y: 0% (left) and 8% prestrain(right) Uni-axial tension Uni-axial tension Cyclic test M125 result ) ( 800 400 -400 -800 Unstrained Uni-axial compression 0.04 0.08 True strain Figure M125-8. Cyclic plasticity verification on one element. ) ( 800 700 600 500 400 300 200 100 Experiment Basic model(SC1=200) Modified model (SC1=2000, SC2=200 in Eq. (1) 0.01 0.02 0.03 0.04 0.05 0.06 True strain Figure M125-9. Effect of SC1 and SC2 (reproduced from the original Yoshida & Uemori’s paper). 1200 900 600 300 -300 -600 -900 -1200 1200 900 600 300 -300 -600 -900 -1200 Experimental result Curve fitting result SC1 + SC2 -0.03 0.03 SC1 only -0.03 0.03 Figure M125-10. Material curve fitting comparison (reproduced from an original color slide courtesy of CYBERNET SYSTEMS CO., LTD.). *MAT_MODIFIED_HONEYCOMB This is Material Type 126. The major use of this material model is for aluminum honeycomb crushable foam materials with anisotropic behavior. Three yield surfaces are available. In the first, nonlinear elastoplastic material behavior can be defined separately for all normal and shear stresses, which are considered to be fully uncoupled. In the second, a yield surface is defined that considers the effects of off-axis loading. The second yield surface is transversely isotropic. A drawback of this second yield surface is that the material can collapse in a shear mode due to low shear resistance. There was no obvious way of increasing the shear resistance without changing the behavior in purely uniaxial compression. Therefore, in the third option, the model has been modified so that the user can prescribe the shear and hydrostatic resistance in the material without affecting the uniaxial behavior. The choice of the second yield surface is flagged by the sign of the first load curve ID, LCA. The third yield surface is flagged by the sign of ECCU, which becomes the initial stress yield limit in simple shear. A description is given below. The development of the second and third yield surfaces are based on experimental test results of aluminum honeycomb specimens at Toyota Motor Corporation. The default element for this material is solid type 0, a nonlinear spring type brick element. The recommended hourglass control is the type 2 viscous formulation for one point integrated solid elements. The stiffness form of the hourglass control when used with this constitutive model can lead to nonphysical results since strain localization in the shear modes can be inhibited. Card 1 1 Variable MID 2 RO Type A8 F 3 E F 4 PR F 5 SIGY F 6 VF F 7 8 MU BULK F F Default none none none none none none .05 0.0 Card 2 1 2 3 4 5 6 7 8 Variable LCA LCB LCC LCS LCAB LCBC LCCA LCSR Type F F F F F F F F Default none LCA LCA LCA LCS LCS LCS optional Card 3 1 2 3 4 5 6 7 8 Variable EAAU EBBU ECCU GABU GBCU GCAU AOPT MACF Type F F F F F F Card 4 Variable 1 XP Type F Card 5 Variable 1 D1 Type F 2 YP F 2 D2 F 3 ZP F 3 D3 F 4 A1 F 4 5 A2 F 5 6 A3 F 6 I 8 7 7 8 TSEF SSEF VREF TREF SHDFLG F F F F F Additional card for AOPT = 3 or AOPT = 4. Card 6 Variable 1 V1 Type F 2 V2 F 3 V3 F 4 5 6 7 *MAT_MODIFIED_HONEYCOMB Card 7 1 2 3 4 5 6 7 8 Variable LCSRA LCSRB LCSRC LCSRAB LCSRBC LCSCA Type F F F F F F VARIABLE DESCRIPTION MID RO E PR SIGY VF Material identification. A unique number or label not exceeding 8 characters must be specified. Mass density. Young’s modulus for compacted honeycomb material. Poisson’s ratio for compacted honeycomb material. Yield stress for fully compacted honeycomb. Relative volume at which the honeycomb is fully compacted. This parameter is ignored for corotational solid elements, types 0 and 9. MU μ, material viscosity coefficient. (default=.05) Recommended. BULK Bulk viscosity flag: EQ.0.0: bulk viscosity is not used. This is recommended. EQ.1.0: bulk viscosity is active and μ = 0. This will give results identical to previous versions of LS-DYNA. LCA Load curve ID, see *DEFINE_CURVE: LCA.LT.0: Yield stress as a function of the angle off the material axis in degrees. LCA.GT.0: sigma-aa versus normal strain component aa. For the corotational solid elements, types 0 and 9, engi- neering strain is expected, but for all other solid el- ement formulations a logarithmic strain is expected. See Remarks. VARIABLE DESCRIPTION LCB Load curve ID, see *DEFINE_CURVE: LCA.LT.0: strong axis hardening stress as a function of the volumetric strain. LCA.GT.0: sigma-bb versus normal strain component bb. For the corotational solid elements, types 0 and 9, engi- neering strain is expected, but for all other solid el- ement formulations a logarithmic strain is expected. Default LCB = LCA. See Remarks. LCC Load curve ID, see *DEFINE_CURVE: LCA.LT.0: weak axis hardening stress as a function of the volumetric strain. LCA.GT.0: sigma-cc versus normal strain component cc. For the corotational solid elements, types 0 and 9, engi- neering strain is expected, but for all other solid el- ement formulations a logarithmic strain is expected. Default LCC = LCA. See Remarks. LCS Load curve ID, see *DEFINE_CURVE: LCA.LT.0: damage curve giving shear stress multiplier as a function of the shear strain component. This curve definition is optional and may be used if damage is desired. IF SHDFLG = 0 (the default), the damage value multiplies the stress every time step and the stress is updated incrementally. The damage curve should be set to unity until failure begins. After failure the value should drop to 0.999 or 0.99 or any number between zero and one depending on how many steps are needed to zero the stress. Alterna- tively, if SHDFLG = 1, the damage value is treated as a factor that scales the shear stress compared to the undamaged value. LCA.GT.0: shear stress versus shear strain. For the corotational solid elements, types 0 and 9, engineering strain is expected, but for all other solid element formula- tions a shear strain based on the deformed configu- Each ration component of shear stress may have its own load curve. See Remarks. Default LCS = LCA. is used. *MAT_MODIFIED_HONEYCOMB DESCRIPTION LCAB Load curve ID, see *DEFINE_CURVE. Default LCAB = LCS: LCA.LT.0: damage curve giving shear ab-stress multiplier as a function of the ab-shear strain component. This curve definition is optional and may be used if damage is desired. See LCS above. LCA.GT.0: sigma-ab versus shear strain-ab. For the corotation- al solid elements, types 0 and 9, engineering strain is expected, but for all other solid element formula- tions a shear strain based on the deformed configu- ration is used. See Remarks. LCBC Load curve ID, see *DEFINE_CURVE. Default LCBC = LCS: LCA.LT.0: damage curve giving bc-shear stress multiplier as a function of the ab-shear strain component. This curve definition is optional and may be used if damage is desired. See LCS above. LCA.GT.0: sigma-bc versus shear strain-bc. For the corotation- al solid elements, types 0 and 9, engineering strain is expected, but for all other solid element formula- tions a shear strain based on the deformed configu- ration is used. See Remarks. LCCA Load curve ID, see *DEFINE_CURVE. Default LCCA = LCS: LCA.LT.0: damage curve giving ca-shear stress multiplier as a function of the ca-shear strain component. This curve definition is optional and may be used if damage is desired. See LCS above. LCA.GT.0: sigma-ca versus shear strain-ca. For the corotational solid elements, types 0 and 9, engineering strain is expected, but for all other solid element formula- tions a shear strain based on the deformed configu- ration is used. See Remarks. LCSR the Load curve ID, see *DEFINE_CURVE, for strain-rate effects defining rate factor versus 𝑖𝑗𝜀′̇ 3 (𝜀′̇ ̇ = √2 scaled using this curve. 𝑖𝑗). This is optional. The curves defined above are effective strain scale 𝜀̅ EAAU Elastic modulus Eaau in uncompressed configuration. VARIABLE DESCRIPTION EBBU ECCU GABU GBCU GCAU Elastic modulus Ebbu in uncompressed configuration. Elastic modulus Eccu in uncompressed configuration. LT.0.0: 𝜎𝑑 𝑌, |ECCU| initial stress limit (yield) in simple shear. Also, LCA < 0 to activate the transversely isotropic yield surface. Shear modulus Gabu in uncompressed configuration. Shear modulus Gbcu in uncompressed configuration. Shear modulus Gcau in uncompressed configuration. ECCU.LT.0.0: 𝜎𝑝 𝑌, GCAU initial stress in hydrostatic compression. Also, LCA < 0 to acti- vate the transversely isotropic yield surface. (yield) limit AOPT Material axes option : EQ.0.0: locally orthotropic with material axes determined by element nodes 1, 2, and 4, as with *DEFINE_COORDI- NATE_NODES. EQ.1.0: locally orthotropic with material axes determined by a point in space and the global location of the element center; this is the a-direction. EQ.2.0: globally orthotropic with material axes determined by vectors defined below, as with *DEFINE_COORDI- NATE_VECTOR. EQ.3.0: locally orthotropic material axes determined by rotating the material axes about the element normal by an angle, BETA, from a line in the plane of the element defined by the cross product of the vector v with the element normal. The plane of a solid element is the midsurface between the inner surface and outer surface defined by the first four nodes and the last four nodes of the connectivity of the element, respectively. EQ.4.0: locally orthotropic in cylindrical coordinate system with the material axes determined by a vector v, and an originating point, p, which define the centerline ax- is. This option is for solid elements only. *MAT_MODIFIED_HONEYCOMB DESCRIPTION LT.0.0: the absolute value of AOPT is a coordinate system ID number (CID on *DEFINE_COORDINATE_NODES, *DEFINE_COORDINATE_SYSTEM or *DEFINE_CO- ORDINATE_VECTOR). MACF Material axes change flag: EQ.1: No change, default, EQ.2: switch material axes a and b, EQ.3: switch material axes a and c, EQ.4: switch material axes b and c. XP YP ZP Coordinates of point p for AOPT = 1 and 4. A1 A2 A3 Components of vector a for AOPT = 2. D1 D2 D3 Components of vector d for AOPT = 2. V1 V2 V3 Define components of vector v for AOPT = 3 and 4. TSEF SSEF 2-680 (EOS) Tensile strain at element failure (element will erode). VARIABLE VREF TREF DESCRIPTION This is an optional input parameter for solid elements types 1, 2, 3, 4, and 10. Relative volume at which the reference geometry is stored. At this time the element behaves like a nonlinear spring. The TREF, below, is reached first then VREF will have no effect. This is an optional input parameter for solid elements types 1, 2, 3, 4, and 10. Element time step size at which the reference geometry is stored. When this time step size is reached the element behaves like a nonlinear spring. If VREF, above, is reached first then TREF will have no effect. SHDFLG Flag defining treatment of damage from curves LCS, LCAB, LCBC and LCCA (relevant only when LCA < 0): LCSRA EQ.0.0: Damage reduces shear stress every time step, EQ.1.0: Damage = (shear stress)/(undamaged shear stress) Optional load curve ID if LCSR = -1, see *DEFINE_CURVE, for strain rate effects defining the scale factor for the yield stress in the a-direction versus the natural logarithm of the absolute value of deviatoric strain rate in the a-direction. This curve is optional. The scale factor for the lowest value of strain rate defined by the curve is used if the strain rate is zero. The scale factor for the highest value of strain rate defined by the curve also defines the upper limit of the scale factor. LCSRB Optional load curve ID if LCSR = -1, see *DEFINE_CURVE, for strain rate effects defining the scale factor for the yield stress in the b-direction versus the natural logarithm of the absolute value of deviatoric strain LCSRC Similar definition as for LCSA and LCSB above. LCSRAB Similar definition as for LCSA and LCSB above. LCSRBC Similar definition as for LCSA and LCSB above. LCSRCA Similar definition as for LCSA and LCSB above. Remarks: For efficiency it is strongly recommended that the load curve ID’s: LCA, LCB, LCC, LCS, LCAB, LCBC, and LCCA, contain exactly the same number of points with corresponding strain values on the abscissa. If this recommendation is followed the cost of the table lookup is insignificant. Conversely, the cost increases significantly if the abscissa strain values are not consistent between load curves. For solid element formulations 1 and 2, the behavior before compaction is orthotropic where the components of the stress tensor are uncoupled, i.e., an a component of strain will generate resistance in the local a-direction with no coupling to the local b and c directions. The elastic moduli vary from their initial values to the fully compacted values linearly with the relative volume: 𝐸𝑎𝑎 = 𝐸𝑎𝑎𝑢 + 𝛽(𝐸 − 𝐸𝑎𝑎𝑢) 𝐸𝑏𝑏 = 𝐸𝑏𝑏𝑢 + 𝛽(𝐸 − 𝐸𝑏𝑏𝑢) 𝐸𝑐𝑐 = 𝐸𝑐𝑐𝑢 + 𝛽(𝐸 − 𝐸𝑐𝑐𝑢) 𝐺𝑎𝑏 = 𝐸𝑎𝑏𝑢 + 𝛽(𝐺 − 𝐺𝑎𝑏𝑢) 𝐺𝑏𝑐 = 𝐺𝑏𝑐𝑢 + 𝛽(𝐺 − 𝐺𝑏𝑐𝑢) 𝐺𝑐𝑎 = 𝐺𝑐𝑎𝑢 + 𝛽(𝐺 − 𝐺𝑐𝑎𝑢) where 𝛽 = max [min ( 1 − 𝑉 1 − 𝑉𝑓 , 1) , 0] and G is the elastic shear modulus for the fully compacted honeycomb material 𝐺 = 2(1 + 𝑣) The relative volume, V, is defined as the ratio of the current volume over the initial volume, and typically, V = 1 at the beginning of a calculation. For corotational solid elements, types 0 and 9, the components of the stress tensor remain uncoupled and the uncompressed elastic moduli are used, that is, the fully compacted elastic moduli are ignored. The load curves define the magnitude of the stress as the material undergoes deformation. The first value in the curve should be less than or equal to zero corresponding to tension and increase to full compaction. Care should be taken when defining the curves so the extrapolated values do not lead to negative yield stresses. At the beginning of the stress update we transform each element’s stresses and strain rates into the local element coordinate system. For the uncompacted material, the trial stress components are updated using the elastic interpolated moduli according to: 𝑛+1trial 𝜎𝑎𝑎 = 𝜎𝑎𝑎 𝑛 + 𝐸𝑎𝑎Δ𝜀𝑎𝑎 𝑛+1trial 𝜎𝑐𝑐 𝑛+1trial 𝜎𝑏𝑏 = 𝜎𝑐𝑐 = 𝜎𝑏𝑏 𝑛 + 𝐸𝑐𝑐Δ𝜀𝑐𝑐 𝑛 + 𝐸𝑏𝑏Δ𝜀𝑏𝑏 𝑛+1trial 𝜎𝑎𝑏 𝑛+1trial 𝜎𝑏𝑐 = 𝜎𝑎𝑏 𝑛 + 2𝐺𝑎𝑏Δ𝜀𝑎𝑏 = 𝜎𝑏𝑐 𝑛 + 2𝐺𝑏𝑐Δ𝜀𝑏𝑐 𝑛+1trial 𝜎𝑐𝑎 = 𝜎𝑐𝑎 𝑛 + 2𝐺𝑐𝑎Δ𝜀𝑐𝑎 If LCA > 0, each component of the updated stress tensor is checked to ensure that it does not exceed the permissible value determined from the load curves, e.g., if then 𝑛+1trial ∣𝜎𝑖𝑗 ∣ > 𝜆𝜎𝑖𝑗(𝜀𝑖𝑗) 𝑛+1 = 𝜎𝑖𝑗(𝜀𝑖𝑗) 𝜎𝑖𝑗 𝑛+1trial 𝜆𝜎𝑖𝑗 𝑛+1trial∣ ∣𝜎𝑖𝑗 On Card 3 𝜎𝑖𝑗(𝜀𝑖𝑗) is defined in the load curve specified in columns 31-40 for the aa stress component, 41-50 for the bb component, 51-60 for the cc component, and 61-70 for the ab, bc, cb shear stress components. The parameter λ is either unity or a value taken from the load curve number, LCSR, that defines λ as a function of strain-rate. Strain- rate is defined here as the Euclidean norm of the deviatoric strain-rate tensor. If LCA < 0, a transversely isotropic yield surface is obtained where the uniaxial limit stress, 𝜎 𝑦(𝜑, 𝜀vol), can be defined as a function of angle 𝜑 with the strong axis and volumetric strain, 𝜀vol. In order to facilitate the input of data to such a limit stress surface, the limit stress is written as: 𝜎 𝑦(𝜑, 𝜀vol) = 𝜎 𝑏(𝜑) + (cos𝜑)2𝜎 𝑠(𝜀vol) + (sin𝜑)2𝜎 𝑤(𝜀vol) where the functions 𝜎 𝑏, 𝜎 𝑠, and 𝜎 𝑤 are represented by load curves LCA, LCB, LCC, respectively. The latter two curves can be used to include the stiffening effects that are observed as the foam material crushes to the point where it begins to lock up. To ensure that the limit stress decreases with respect to the off-angle the curves should be defined such that following equations hold: and ∂𝜎 𝑏(𝜑) ∂𝜑 ≤ 0 𝜎 𝑠(𝜀vol) − 𝜎 𝑤(𝜀vol) ≥ 0. A drawback of this implementation was that the material often collapsed in shear mode due to low shear resistance. There was no way of increasing the shear resistance without changing the behavior in pure uniaxial compression. We have therefore modified the model so that the user can optionally prescribe the shear and hydrostatic resistance in the material without affecting the uniaxial behavior. We introduce the 𝑌(𝜀vol) as the hydrostatic and shear limit stresses, respectively. parameters 𝜎𝑝 These are functions of the volumetric strain and are assumed given by 𝑌(𝜀vol) and 𝜎𝑑 𝑌(𝜀vol) = 𝜎𝑝 𝜎𝑝 𝑌(𝜀vol) = 𝜎𝑑 𝜎𝑑 𝑌 + 𝜎 𝑠(𝜀vol) , 𝑌 + 𝜎 𝑠(𝜀vol) where we have reused the densification function 𝜎 𝑠. The new parameters are the initial 𝑌, and are provided by the user as hydrostatic and shear limit stress values, 𝜎𝑝 GCAU and |ECCU|, respectively. The negative sign of ECCU flags the third yield 𝑌 and 𝜎𝑑 𝑌(𝜀vol) and (iii) for a simple shear the stress limit is given by 𝜎𝑑 surface option whenever LCA < 0. The effect of the third formulation is that (i) for a uniaxial stress the stress limit is given by 𝜎 𝑌(𝜙, 𝜀vol), (ii) for a pressure the stress limit is 𝑌(𝜀vol). given by 𝜎𝑝 Experiments have shown that the model may give noisy responses and inhomogeneous deformation modes if parameters are not chosen with care. We therefore recommend to (i) avoid large slopes in the function 𝜎 𝑃, (ii) let the functions 𝜎 𝑠 and 𝜎 𝑤 be slightly increasing and (iii) avoid large differences between the stress limit values 𝜎 𝑦(𝜑, 𝜀vol), 𝑌(𝜀vol). These guidelines are likely to contradict how one would 𝑌(𝜀vol) and 𝜎𝑑 𝜎𝑝 interpret test data and it is up to the user to find a reasonable trade-off between matching experimental results and avoiding the mentioned numerical side effects. For fully compacted material (element formulations 1 and 2), we assume that the material behavior is elastic-perfectly plastic and updated the stress components according to: trial = 𝑠𝑖𝑗 𝑠𝑖𝑗 𝑛 + 2𝐺Δ𝜀𝑖𝑗 𝑑𝑒𝑣𝑛+1 2⁄ where the deviatoric strain increment is defined as Δ𝜀𝑖𝑗 𝑑𝑒𝑣 = Δ𝜀𝑖𝑗 − Δ𝜀𝑘𝑘𝛿𝑖𝑗. We now check to see if the yield stress for the fully compacted material is exceeded by comparing trial = ( 𝑠eff 2⁄ trial) trial𝑠𝑖𝑗 𝑠𝑖𝑗 the effective trial stress to the yield stress, σy (Card 1, field 41-50). If the effective trial stress exceeds the yield stress we simply scale back the stress components to the yield surface We can now update the pressure using the elastic bulk modulus, K 𝑛+1 = 𝑠𝑖𝑗 𝜎𝑦 trial 𝑠eff trial. 𝑠𝑖𝑗 𝑛+1 𝑝𝑛+1 = 𝑝𝑛 − 𝐾Δ𝜀𝑘𝑘 2⁄ 𝐾 = 3(1 − 2𝑣) and obtain the final value for the Cauchy stress 𝑛+1 = 𝑠𝑖𝑗 𝜎𝑖𝑗 𝑛+1 − 𝑝𝑛+1𝛿𝑖𝑗 After completing the stress update we transform the stresses back to the global configuration. For *CONSTRAINED_TIED_NODES_WITH_FAILURE, the failure is based on the volume strain instead to the plastic strain. Curve extends into negative strain quadrant since LS-DYNA will extrapolate using the two end points. It is important that the extropolation does not extend into the negative stress region. σ ij unloading and reloading path Strain: -ε ij Unloading is based on the interpolated Young’s moduli which must provide an unloading tangent that exceeds the loading tangent. Figure M126-1. Stress versus strain. Note that the “yield stress” at a strain of zero is nonzero. In the load curve definition the “time” value is the directional strain and the “function” value is the yield stress. Note that for element types 0 and 9 engineering strains are used, but for all other element types the rates are integrated in time. *MAT_ARRUDA_BOYCE_RUBBER This is Material Type 127. This material model provides a hyperelastic rubber model, see [Arruda and Boyce 1993] combined optionally with linear viscoelasticity as outlined by [Christensen 1980]. Card 1 1 Variable MID Type A8 Card 2 1 2 RO F 2 3 K F 3 Variable LCID TRAMP NT Type F F F 4 G F 4 5 N F 5 6 7 8 6 7 8 Viscoelastic Constant Cards. Up to 6 cards may be input. A keyword card (with a “*” in column 1) terminates this input if less than 6 cards are used. Card 3 Variable Type 1 GI F VARIABLE MID 2 3 4 5 6 7 8 BETAI F DESCRIPTION Material identification. A unique number or label not exceeding 8 characters must be specified. RO Mass density K G N Bulk modulus Shear modulus Number of statistical links VARIABLE LCID DESCRIPTION Optional load curve ID of relaxation curve if constants βI are determined via a least squares fit. This relaxation curve is shown in Figure M76-1. This model ignores the constant stress. TRAMP Optional ramp time for loading. NT Number of Prony series terms in optional fit. If zero, the default is 6. Currently, the maximum number is 6. Values less than 6, possibly 3-5 are recommended, since each term used adds significantly to the cost. Caution should be exercised when taking the results from the fit. Always check the results of the fit in the output file. Preferably, all generated coefficients should be positive. Negative values may lead to unstable results. Once a satisfactory fit has been achieved it is recommended that the coefficients which are written into the output file be input in future runs. GI Optional shear relaxation modulus for the ith term. BETAI Optional decay constant if ith term. Remarks: Rubber is generally considered to be fully incompressible since the bulk modulus greatly exceeds the shear modulus in magnitude. To model the rubber as an unconstrained material a hydrostatic work term, 𝑊𝐻(𝐽), is included in the strain energy functional which is function of the relative volume, J, [Ogden 1984]: 𝑊(𝐽1, 𝐽2, 𝐽) = 𝑛𝑘𝜃 [ (𝐽1 − 3) + 20𝑁 2 − 9) + (𝐽1 + 𝑛𝑘𝜃 [ 19 7000𝑁3 (𝐽1 4 − 81) + 3 − 27)] 11 1050𝑁2 (𝐽1 519 673750𝑁4 (𝐽1 5 − 243)] + 𝑊𝐻(𝐽) where the hydrostatic work term is in terms of the bulk modulus, K, and the third invariant, J, as: Rate effects are taken into account through linear viscoelasticity by a convolution integral of the form: 𝑊𝐻(𝐽) = (𝐽 − 1)2 𝜎𝑖𝑗 = ∫ 𝑔𝑖𝑗𝑘𝑙(𝑡 − 𝜏) ∂𝜀𝑘𝑙 ∂𝜏 𝑑𝜏 or in terms of the second Piola-Kirchhoff stress, 𝑆𝑖𝑗, and Green's strain tensor, 𝐸𝑖𝑗, 𝑆𝑖𝑗 = ∫ 𝐺𝑖𝑗𝑘𝑙 (𝑡 − 𝜏) ∂𝐸𝑘𝑙 ∂𝜏 𝑑𝜏 where 𝑔𝑖𝑗𝑘𝑙(𝑡 − 𝜏) and 𝐺𝑖𝑗𝑘𝑙(𝑡 − 𝜏) are the relaxation functions for the different stress measures. This stress is added to the stress tensor determined from the strain energy functional. If we wish to include only simple rate effects, the relaxation function is represented by six terms from the Prony series: given by, 𝑔(𝑡) = 𝛼0 + ∑ 𝛼𝑚𝑒−𝛽𝑡 𝑚=1 𝑔(𝑡) = ∑ 𝐺𝑖𝑒−𝛽𝑖𝑡 𝑖=1 This model is effectively a Maxwell fluid which consists of a dampers and springs in series. We characterize this in the input by shear moduli, 𝐺𝑖, and decay constants, 𝛽𝑖. The viscoelastic behavior is optional and an arbitrary number of terms may be used. *MAT_128 This is Material Type 128. This material model provides a heart tissue model described in the paper by Walker et al [2005] as interpreted by Kay Sun. It is backward compatible with an earlier heart tissue model described in the paper by Guccione, McCulloch, and Waldman [1991]. Both models are transversely isotropic. Card 1 1 Variable MID 2 RO Type A8 F 3 C F 4 B1 F 5 B2 F 6 B3 F 7 P F 8 B F Skip to Card 3 to activate older Guccione, McCulloch, and Waldman [1991] model. Card 2 Variable 1 L0 2 3 CA0MAX LR 4 M 5 BB 6 7 8 CA0 TMAX TACT Type F Card 3 1 I 2 Variable AOPT MACF Type F I 3 4 5 6 7 8 Card 4 Variable 1 XP Type F 2 YP F 3 ZP F 4 A1 F 5 A2 F 6 A3 F 7 Variable 1 V1 Type F VARIABLE MID *MAT_HEART_TISSUE 2 V2 F 3 V3 F 4 D1 F 5 D2 F 6 D3 F 7 8 BETA F DESCRIPTION Material identification. A unique number or label not exceeding 8 characters must be specified. RO Mass density C B1 B2 B3 P B L0 Diastolic material coefficient. 𝑏1, diastolic material coefficient. 𝑏2, diastolic material coefficient. 𝑏3, diastolic material coefficient. Pressure in the muscle tissue Systolic material coefficient. Omit for the earlier model. 𝑙0, sacromere length at which no active tension develops. Omit for the earlier model. CA0MAX (𝐶𝑎0)max, maximum peak intracellular calcium concentrate. Omit for the earlier model. LR M BB CA0 TMAX TACT 𝑙𝑅, Stress-free sacromere length. Omit for the earlier model. Systolic material coefficient. Omit for the earlier model. Systolic material coefficient. Omit for the earlier model. 𝐶𝑎0, peak intracellular calcium concentration. Omit for the earlier model. 𝑇max, maximum isometric tension achieved at the longest sacromere length. Omit for the earlier model. 𝑡act, time at which active contraction initiates. Omit for the earlier model VARIABLE AOPT DESCRIPTION Material axes option : EQ.0.0: locally orthotropic with material axes determined by element nodes 1, 2, and 4, as with *DEFINE_COORDI- NATE_NODES. EQ.1.0: locally orthotropic with material axes determined by a point in space and the global location of the element center; this is the a-direction. EQ.2.0: globally orthotropic with material axes determined by vectors defined below, as with *DEFINE_COORDI- NATE_VECTOR. EQ.3.0: locally orthotropic material axes determined by rotating the material axes about the element normal by an angle, BETA, from a line in the plane of the element defined by the cross product of the vector v with the element normal. EQ.4.0: locally orthotropic in cylindrical coordinate system with the material axes determined by a vector v, and an originating point, P, which define the centerline ax- is. LT.0.0: the absolute value of AOPT is a coordinate system ID number (CID on *DEFINE_COORDINATE_NODES, *DEFINE_COORDINATE_SYSTEM or *DEFINE_CO- ORDINATE_VECTOR). Available in R3 version of 971 and later. MACF Material axes change flag for brick elements: EQ.1: No change, default, EQ.2: switch material axes a and b, EQ.3: switch material axes a and c, EQ.4: switch material axes b and c. XP, YP, ZP xp yp zp, define coordinates of point p for AOPT = 1 and 4. A1, A2, A3 a1 a2 a3, define components of vector a for AOPT = 2. D1, D2, D3 d1 d2 d3, define components of vector d for AOPT = 2. V1, V2, V3 v1 v2 v3, define components of vector v for AOPT = 3 and 4. Material angle in degrees for AOPT = 3, may be overridden on the element card, see *ELEMENT_SOLID_ORTHO. *MAT_128 VARIABLE BETA Remarks: 1. The tissue model is described in terms of the energy functional that is transversely isotropic with respect to the local fiber direction, (𝑒𝑄 − 1) 𝑊 = 𝑄 = 𝑏𝑓 𝐸11 2 + 𝑏𝑡(𝐸22 2 + 𝐸33 2 + 𝐸23 2 + 𝐸32 2 ) + 𝑏𝑓𝑠(𝐸12 2 + 𝐸21 2 + 𝐸13 2 + 𝐸31 2 ) with 𝐶, 𝑏𝑓 , 𝑏𝑡, and 𝑏𝑓𝑠 material parameters and E the Lagrange-Green strains. The systolic contraction was modeled as the sum of the passive stress derived from the strain energy function and an active fiber directional component, 𝑇0, which is a function of time, t, − 𝑝𝐽𝐶−1 + 𝑇0{𝑡, 𝐶𝑎0, 𝑙} 𝑆 = 𝜎 = ∂𝑊 ∂𝐸 𝐹𝑆𝐹𝑇 with 𝑆 the second Piola-Kirchoff stress tensor, 𝐶 the right Cauchy-Green de- formation tensor, J the Jacobian of the deformation gradient tensor 𝐹, and 𝜎 the Cauchy stress tensor. The active fiber directional stress component is defined by a time-varying elas- tance model, which at end-systole, is reduced to 𝑇0 = 𝑇max 𝐶𝑎0 2 + 𝐸𝐶𝑎50 2 𝐶𝑡 𝐶𝑎0 with 𝑇max the maximum isometric tension achieved at the longest sacromere length and maximum peak intracellular calcium concentration. The length- dependent calcium sensitivity and internal variable is given by, 𝐸𝐶𝑎50 = (𝐶𝑎0)max √exp[𝐵(𝑙 − 𝑙0] − 1 𝐶𝑡 = 1/2(1 − cos 𝑤) 𝑙 = 𝑙𝑅√2𝐸11 + 1 𝑤 = 𝜋 0.25 + 𝑡𝑟 𝑡𝑟 𝑡𝑟 = 𝑚𝑙 + 𝑏𝑏 A cross-fiber, in-plane stress equivalent to 40% of that along the myocardial fiber direction is added. 2. The earlier tissue model is described in terms of the energy functional in terms of the Green strain components, 𝐸𝑖𝑗, 𝑊(𝐸) = (𝑒𝑄 − 1) + 𝑄 = 𝑏1𝐸11 2 + 𝐸33 2 + 𝑏2(𝐸22 𝑃(𝐼3 − 1) 2 + 𝐸23 2 + 𝐸32 2 ) + 𝑏3(𝐸12 2 + 𝐸21 2 + 𝐸13 2 + 𝐸31 2 ) The Green components are modified to eliminate any effects of volumetric work following the procedures of Ogden. See the paper by Guccione et al [1991] for more detail. *MAT_LUNG_TISSUE This is Material Type 129. This material model provides a hyperelastic model for heart tissue, see [Vawter 1980] combined optionally with linear viscoelasticity as outlined by [Christensen 1980]. Card 1 1 Variable MID 2 RO Type A8 F Card 2 Variable 1 C1 Type F 2 C2 F 3 K F 3 4 C F 4 5 6 7 8 DELTA ALPHA BETA F 5 F 6 F 7 8 LCID TRAMP NT F F F Viscoelastic Constant Cards. Up to 6 cards may be input. A keyword card (with a “*” in column 1) terminates this input if less than 6 cards are used. Card 3 Variable Type 1 GI F 2 3 4 5 6 7 8 BETAI F VARIABLE DESCRIPTION MID RO K C Material identification. A unique number or label not exceeding 8 characters must be specified. Mass density Bulk modulus Material coefficient. DELTA Δ, material coefficient. ALPHA 𝛼, material coefficient. VARIABLE DESCRIPTION BETA 𝛽, material coefficient. C1 C2 Material coefficient. Material coefficient. LCID Optional load curve ID of relaxation curve If constants 𝐺𝑖 and 𝛽𝑖 are determined via a least squares fit. This relaxation curve is shown in Figure M76-1. This model ignores the constant stress. TRAMP Optional ramp time for loading. NT Number of Prony series terms in optional fit. If zero, the default is 6. Currently, the maximum number is 6. Values less than 6, possibly 3 - 5 are recommended, since each term used adds significantly to the cost. Caution should be exercised when taking the results from the fit. Always check the results of the fit in the output file. Preferably, all generated coefficients should be positive. Negative values may lead to unstable results. Once a satisfactory fit has been achieved it is recommended that the coefficients which are written into the output file be input in future runs. Gi Optional shear relaxation modulus for the ith term BETAi Optional decay constant if ith term Remarks: The material is described by a strain energy functional expressed in terms of the invariants of the Green Strain: 𝑊(𝐼1, 𝐼2) = 2Δ 𝑒(𝛼𝐼1 2+𝛽𝐼2) + 12𝐶1 Δ(1 + 𝐶2) [𝐴(1+𝐶2) − 1] 𝐴2 = (𝐼1 + 𝐼2) − 1 where the hydrostatic work term is in terms of the bulk modulus, K, and the third invariant, J, as: 𝑊𝐻(𝐽) = (𝐽 − 1)2 Rate effects are taken into account through linear viscoelasticity by a convolution integral of the form: 𝜎𝑖𝑗 = ∫ 𝑔𝑖𝑗𝑘𝑙 (𝑡 − 𝜏) ∂𝜀𝑘𝑙 ∂𝜏 𝑑𝜏 or in terms of the second Piola-Kirchhoff stress, 𝑆𝑖𝑗, and Green's strain tensor, 𝐸𝑖𝑗, 𝑆𝑖𝑗 = ∫ 𝐺𝑖𝑗𝑘𝑙 (𝑡 − 𝜏) ∂ 𝐸𝑘𝑙 ∂𝜏 𝑑𝜏 where 𝑔𝑖𝑗𝑘𝑙(𝑡 − 𝜏) and 𝐺𝑖𝑗𝑘𝑙(𝑡 − 𝜏) are the relaxation functions for the different stress measures. This stress is added to the stress tensor determined from the strain energy functional. If we wish to include only simple rate effects, the relaxation function is represented by six terms from the Prony series: given by, 𝑔(𝑡) = 𝛼0 + ∑ 𝛼𝑚 𝑚=1 𝑒−𝛽 𝑡 𝑔(𝑡) = ∑ 𝐺𝑖𝑒−𝛽𝑖 𝑡 𝑖=1 This model is effectively a Maxwell fluid which consists of a dampers and springs in series. We characterize this in the input by shear moduli, 𝐺𝑖, and decay constants, 𝛽𝑖. The viscoelastic behavior is optional and an arbitrary number of terms may be used. *MAT_130 This is Material Type 130. This model is available the Belytschko-Tsay and the C0 triangular shell elements and is based on a resultant stress formulation. In-plane behavior is treated separately from bending in order to model perforated materials such as television shadow masks. If other shell formulations are specified, the formulation will be automatically switched to Belytschko-Tsay. As implemented, this material model cannot be used with user defined integration rules. NOTE: This material does not support specification of a ma- terial angle, 𝛽𝑖, for each through-thickness integra- tion point of a shell. Card 1 1 Variable MID Type A8 Card 2 1 2 RO F 2 3 YS F 3 4 EP F 4 5 6 7 8 5 6 7 8 Variable E11P E22P V12P V21P G12P G23P G31P Type F Card 3 1 F 2 F 3 F 4 F 5 F 6 F 7 8 Variable E11B E22B V12B V21B G12B AOPT Type F Card 4 1 F 2 F 3 Variable Type F F F 4 A1 F 5 A2 F 6 A3 F 7 Variable 1 V1 Type F *MAT_SPECIAL_ORTHOTROPIC 2 V2 F 3 V3 F 4 D1 F 5 D2 F 6 D3 F 7 8 BETA F VARIABLE DESCRIPTION MID RO YS EP E11P E22P V12P V11P G12P G23P G31P E11B E22B V12B V21B G12B Material identification. A unique number or label not exceeding 8 characters must be specified. Mass density. Yield stress. This parameter is optional and is approximates the yield condition. Set to zero if the behavior is elastic. Plastic hardening modulus. 𝐸11𝑝, for in plane behavior. 𝐸22𝑝, for in plane behavior. 𝜈12𝑝, for in plane behavior. 𝜈11𝑝, for in plane behavior. 𝐺12𝑝, for in plane behavior. 𝐺23𝑝, for in plane behavior. 𝐺31𝑝, for in plane behavior. 𝐸11𝑝, for bending behavior. 𝐸22𝑝, for bending behavior. 𝜈12𝑏, for bending behavior. 𝜈21𝑏, for bending behavior. 𝐺12𝑏, for bending behavior. VARIABLE AOPT DESCRIPTION Material axes option : EQ.0.0: locally orthotropic with material axes determined by element nodes 1, 2, and 4, as with *DEFINE_COORDI- NATE_NODES, and then rotated about the shell ele- ment normal by an angle BETA. EQ.2.0: globally orthotropic with material axes determined by vectors defined below, as with *DEFINE_COORDI- NATE_VECTOR. EQ.3.0: locally orthotropic material axes determined by rotating the material axes about the element normal by an angle, BETA, from a line in the plane of the element defined by the cross product of the vector 𝐯 with the element normal. LT.0.0: the absolute value of AOPT is a coordinate system ID number (CID on *DEFINE_COORDINATE_NODES, *DEFINE_COORDINATE_SYSTEM or *DEFINE_CO- ORDINATE_VECTOR). Available in R3 version of 971 and later. A1, A2, A3 (𝑎1, 𝑎2, 𝑎3), define components of vector 𝐚 for AOPT = 2. D1, D2, D3 (𝑑1, 𝑑2, 𝑑3), define components of vector 𝐝 for AOPT = 2. V1 ,V2, V3 (𝑣1, 𝑣2, 𝑣3), define components of vector 𝐯 for AOPT = 3. BETA Material angle in degrees for AOPT = 0 and 3, may be overridden on the element card, see *ELEMENT_SHELL_BETA. Remarks: The in-plane elastic matrix for in-plane, plane stress behavior is given by: 𝐂in plane = 𝑄11𝑝 𝑄12𝑝 0 0 0 ⎤ 𝑄12𝑝 𝑄22𝑝 0 0 0 ⎥ ⎥ 0 0 𝑄44𝑝 0 0 ⎥ ⎥ 0 0 0 𝑄55𝑝 0 ⎥ 0 0 0 0 𝑄66𝑝⎦ ⎡ ⎢ ⎢ ⎢ ⎢ ⎢ ⎣ The terms 𝑄𝑖𝑗𝑝 are defined as: 𝑄11𝑝 = 𝑄22𝑝 = 𝑄12𝑝 = 𝐸11𝑝 1 − 𝜈12𝑝𝜈21𝑝 𝐸22𝑝 1 − 𝜈12𝑝𝜈21𝑝 𝜈12𝑝𝐸11𝑝 1 − 𝜈12𝑝𝜈21𝑝 𝑄44𝑝 = 𝐺12𝑝 𝑄55𝑝 = 𝐺23𝑝 𝑄66𝑝 = 𝐺31𝑝 The elastic matrix for bending behavior is given by: 𝐂bending = 𝑄11𝑏 𝑄12𝑏 0 ⎤ ⎡ 𝑄12𝑏 𝑄22𝑏 0 ⎥ ⎢ 0 0 𝑄44𝑏⎦ ⎣ The terms 𝑄𝑖𝑗𝑝 are similarly defined. Because this is a resultant formulation, nothing is written to the six stress slots of d3plot. Resultant forces and moments may be written to elout and to dynain in place of the six stresses. The first two extra history variables may be used to complete output of the eight resultants to elout and dynain. *MAT_ISOTROPIC_SMEARED_CRACK This is Material Type 131. This model was developed by Lemmen and Meijer [2001] as a smeared crack model for isotropic materials. This model is available of solid elements only and is restricted to cracks in the x-y plane. Users should choose other models unless they have the report by Lemmen and Meijer [2001]. Card 1 1 Variable MID 2 RO Type A8 F 3 E F 4 PR F 5 6 ISPL SIGF I F 7 GK F 8 SR F VARIABLE DESCRIPTION MID RO E PR Material identification. A unique number or label not exceeding 8 characters must be specified. Mass density Young’s modulus Poisson’s ratio ISPL Failure option: EQ.0: Maximum principal stress criterion EQ.5: Smeared crack model EQ.6: Damage model based on modified von Mises strain SIGF Peak stress. GK SR Critical energy release rate. Strength ratio. Remarks: The following documentation is taken nearly verbatim from the documentation of Lemmen and Meijer [2001]. Three methods are offered to model progressive failure. The maximum principal stress criterion detects failure if the maximum (most tensile) principal stress exceeds 𝜎max. Upon failure, the material can no longer carry stress. The second failure model is the smeared crack model with linear softening stress-strain using equivalent uniaxial strains. Failure is assumed to be perpendicular to the principal strain directions. A rotational crack concept is employed in which the crack directions are related to the current directions of principal strain. Therefore crack directions may rotate in time. Principal stresses are expressed as E̅̅̅̅̅1 ⎡ ⎢⎢ ⎣ E̅̅̅̅̅1𝜀̃1 ⎟⎟⎟⎞ E̅̅̅̅̅2𝜀̃2 E̅̅̅̅̅3𝜀̃3⎠ ⎤ ⎥⎥ E̅̅̅̅̅3⎦ 𝜎1 𝜎2 𝜎3⎠ 𝜀̃1 𝜀̃2 𝜀̃3⎠ E̅̅̅̅̅2 (131.1) ⎟⎟⎞ = ⎟⎞ = ⎜⎜⎜⎛ ⎝ ⎜⎜⎛ ⎝ ⎜⎛ ⎝ with E̅̅̅̅̅1, E̅̅̅̅̅2 and E̅̅̅̅̅3 secant stiffness in the terms that depend on internal variables. In the model developed for DYCOSS it has been assumed that there is no interaction between the three directions in which case stresses simply follow from 𝜎𝑗(𝜀̃𝑗) = ⎧E𝜀̃𝑗 {{{ ⎨ {{{ ⎩ 𝜎̅̅̅̅̅ (1 − 𝑖𝑓 0 ≤ 𝜀̃𝑗 ≤ 𝜀̃𝑗,ini 𝜀̃𝑗 − 𝜀̃𝑗,ini 𝜀̃𝑗,ult − 𝜀̃𝑗,ini ) 𝑖𝑓 𝜀̃𝑗,ini < 𝜀̃𝑗 ≤ 𝜀̃𝑗,ult (131.2) 𝑖𝑓 𝜀̃𝑗 > 𝜀̃𝑗,ult with 𝜎̅̅̅̅̅ the ultimate stress, 𝜀̃𝑗,inithe damage threshold, and 𝜀̃𝑗,ultthe ultimate strain in j- direction. The damage threshold is defined as 𝜀̃𝑗,ini = 𝜎̅̅̅̅̅ (131.3) The ultimate strain is obtained by relating the crack growth energy and the dissipated energy ∫ ∫ 𝜎̅̅̅̅̅𝑑𝜀̃𝑗,ult𝑑𝑉 = 𝐺𝐴 (131.4) with G the energy release rate, V the element volume and A the area perpendicular to the principal strain direction. The one point elements LS-DYNA have a single integration point and the integral over the volume may be replaced by the volume. For linear softening it follows 𝜀̃𝑗,ult = 2𝐺𝐴 𝑉𝜎̅̅̅̅̅ (131.5) The above formulation may be regarded as a damage equivalent to the maximum principle stress criterion. The third model is a damage model represented by Brekelmans et. al [1991]. Here the Cauchy stress tensor 𝜎 is expressed as 𝜎 = (1 − 𝐷)E𝜀 (131.6) where D represents the current damage and the factor (1-D) is the reduction factor caused by damage. The scalar damage variable is expressed as function of a so-called damage equivalent strain 𝜀𝑑 𝐷 = 𝐷(𝜀𝑑) = 1 − 𝜀ini(𝜀ult − 𝜀𝑑) 𝜀𝑑(𝜀ult − 𝜀ini) and 𝜀𝑑 = 𝑘 − 1 2𝑘(1 − 2𝑣) 𝐽1 + 2𝑘 √( 𝑘 − 1 1 − 2𝑣 𝐽1) + 6𝑘 (1 + 𝑣)2 𝐽2 (131.7) (131.8) where the constant k represents the ratio of the strength in tension over the strength in compression 𝑘 = 𝜎ult ,tension 𝜎ult, compression (131.9) J1 resp. J2 are the first and second invariant of the strain tensor representing the volumetric and the deviatoric straining respectively 𝐽1 = tr(𝜀) 𝐽2 = tr(𝜀 ⋅ 𝜀) − [𝑡𝑟(𝜀)]2 (131.10) If the compression and tension strength are equal the dependency on the volumetric strain vanishes in (8) and failure is shear dominated. If the compressive strength is much larger than the strength in tension, k becomes small and the J1 terms in (131.8) dominate the behavior. *MAT_ORTHOTROPIC_SMEARED_CRACK This is Material Type 132. This material is a smeared crack model for orthotropic materials. Card 1 1 Variable MID Type A8 Card 2 1 2 RO F 2 3 EA F 3 4 EB F 4 5 EC F 5 6 7 8 PRBA PRCA PRCB F 6 F 7 F 8 Variable UINS UISS CERRMI CERRMII IND ISD Type F Card 3 1 F 2 F 3 F 4 Variable GAB GBC GCA AOPT Type F F F F Card 4 Variable 1 XP Type F Card 5 Variable 1 V1 Type F 2 YP F 2 V2 F 3 ZP F 3 V3 F 4 A1 F 4 D1 F I 5 5 A2 F 5 D2 F I 6 6 A3 F 6 D3 F 7 8 7 8 MACF I 7 8 BETA REF F VARIABLE DESCRIPTION MID RO EA EB EC PRBA PRCA PRCB UINS UISS Material identification. A unique number or label not exceeding 8 characters must be specified. Mass density. Ea, Young’s modulus in a-direction. Eb, Young’s modulus in b-direction. Ec, Young’s modulus in c-direction ba, Poisson’s ratio ba. νca, Poisson’s ratio ca. cb, Poisson’s ratio cb. Ultimate interlaminar normal stress. Ultimate interlaminar shear stress. CERRMI Critical energy release rate mode I CERRMII Critical energy release rate mode II IND Interlaminar normal direction : EQ.1.0: Along local a axis EQ.2.0: Along local b axis EQ.3.0: Along local c axis ISD Interlaminar shear direction : EQ.4.0: Along local ab axis EQ.5.0: Along local bc axis EQ.6.0: Along local ca axis GAB GBC GCA Gab, shear modulus ab. Gbc, shear modulus bc. Gca, shear modulus ca. *MAT_ORTHOTROPIC_SMEARED_CRACK DESCRIPTION AOPT Material axes option, see Figure 2.1. EQ.0.0: locally orthotropic with material axes determined by element nodes as shown in Figure 2.1. Nodes 1, 2, and 4 of an element are identical to the nodes used for the definition of a coordinate system as by *DEFINE_CO- ORDINATE_NODES. EQ.1.0: locally orthotropic with material axes determined by a point in space and the global location of the element center; this is the a-direction. This option is for solid elements only. EQ.2.0: globally orthotropic with material axes determined by vectors defined below, as with *DEFINE_COORDI- NATE_VECTOR. EQ.3.0: locally orthotropic material axes determined by rotating the material axes about the element normal by an angle, BETA, from a line in the plane of the element defined by the cross product of the vector v with the element normal. The plane of a solid element is the midsurface between the inner surface and outer surface defined by the first four nodes and the last four nodes of the connectivity of the element, respectively. EQ.4.0: locally orthotropic in cylindrical coordinate system with the material axes determined by a vector v, and an originating point, P, which define the centerline ax- is. This option is for solid elements only. LT.0.0: the absolute value of AOPT is a coordinate system ID number (CID on *DEFINE_COORDINATE_NODES, *DEFINE_COORDINATE_SYSTEM or *DEFINE_CO- ORDINATE_VECTOR). Available in R3 version of 971 and later. XP YP ZP Define coordinates of point p for AOPT = 1 and 4. A1 A2 A3 Define components of vector a for AOPT = 2. VARIABLE DESCRIPTION MACF Material axes change flag for brick elements: EQ.1: No change, default, EQ.2: switch material axes a and b, EQ.3: switch material axes a and c, EQ.4: switch material axes b and c. V1 V2 V3 Define components of vector v for AOPT = 3 and 4. D1 D2 D3 Define components of vector d for AOPT = 2: BETA REF Material angle in degrees for AOPT = 3, may be overridden on the element card, see *ELEMENT_SOLID_ORTHO. Use reference geometry to initialize the stress tensor. The reference geometry is defined by the keyword: *INITIAL_- FOAM_REFERENCE_GEOMETRY . EQ.0.0: off, EQ.1.0: on. Remarks: This is an orthotropic material with optional delamination failure for brittle composites. The elastic formulation is identical to the DYNA3D model that uses total strain formulation. The constitutive matrix C that relates to global components of stress to the global components of strain is defined as: C = T𝑇C𝐿T where T is the transformation matrix between the local material coordinate system and the global system and C𝐿is the constitutive matrix defined in terms of the material constants of the local orthogonal material axes a, b, and c . Failure is described using linear softening stress strain curves for interlaminar normal and interlaminar shear direction. The current implementation for failure is essentially 2-D. Damage can occur in interlaminar normal direction and a single interlaminar shear direction. The orientation of these directions w.r.t. the principal material directions have to be specified by the user. Based on specified values for the ultimate stress and the critical energy release rate bounding surfaces are defined 𝑓𝑛 = 𝜎𝑛 − 𝜎̅̅̅̅̅𝑛(𝜀𝑛) 𝑓𝑠 = 𝜎𝑠 − 𝜎̅̅̅̅̅𝑠(𝜀𝑠) where the subscripts n and s refer to the normal and shear component. If stresses exceed the bounding surfaces inelastic straining occurs. The ultimate strain is obtained by relating the crack growth energy and the dissipated energy. For solid elements with a single integration point it can be derived 𝜀𝑖,ult = 2𝐺𝑖𝐴 𝑉𝜎𝑖,ult with 𝐺𝑖the critical energy release rate, 𝑉the element volume, A the area perpendicular to the active normal direction and 𝜎𝑖, ult the ultimate stress. For the normal component failure can only occur under tensile loading. For shear component the behavior is symmetric around zero. The resulting stress bounds are depicted in Figure M132-1. Unloading is modeled with a Secant stiffness. n,ult ult Figure M132-1. Shows stress bounds for the active normal component (left) and the archive shear component (right). -τ ult *MAT_133 This is Material Type 133. This model was developed by Barlat et al. [2003] to overcome some shortcomings of the six parameter Barlat model implemented as material 33 (MAT_BARLAT_YLD96) in LS-DYNA. This model is available for shell elements only. Card 1 1 Variable MID 2 RO Type A8 F Card 2 Variable Type 1 K F 2 E0 F 3 E F 3 N F 4 PR F 4 C F 5 FIT F 5 P F 6 7 8 BETA ITER ISCALE F 8 F 6 HARD F F 7 A F Chaboche-Roussilier Card. Additional Card for A < 0. Card 3 1 2 3 4 5 6 7 8 Variable CRC1 CRA1 CRC2 CRA2 CRC3 CRA3 CRC4 CRA4 Type F F F F F F F F Direct Material Parameter Card. Additional card for FIT = 0. Card 4 1 2 3 4 5 6 7 8 Variable ALPHA1 ALPHA2 ALPHA3 ALPHA4 ALPHA5 ALPHA6 ALPHA7 ALPHA8 Type F F F F F F F Test Data Card 1. Additional Card for FIT = 1. Card 5 1 2 3 4 5 6 7 8 Variable SIG00 SIG45 SIG90 R00 R45 R90 Type F F F F F F Test Data Card 2. Additional Card for FIT = 1. Card 6 1 2 3 4 5 6 7 8 Variable SIGXX SIGYY SIGXY DXX DYY DXY Type F F F F F F Hansel Hardening Card 1. Additional Card for HARD = 3. Card 7 Variable 1 CP Type F 2 T0 F 3 4 5 6 7 8 TREF TA0 F F Hansel Hardening Card 2. Additional Card for HARD = 3. Card 8 Variable Type 1 A F 2 B F 3 C F 4 D F 5 P F 6 Q F 7 8 E0MART VM0 F F Hansel Hardening Card 3. Additional Card for HARD = 3. Card 9 1 2 Variable AHS BHS Type F F 3 M F 4 N F 5 6 EPS0 HMART F F 7 K1 F 8 K2 Card 10 1 2 3 4 5 6 7 8 Variable AOPT OFFANG P4 HTFLAG HTA HTB HTC HTD Type F Card 11 1 Variable Type Card 12 Variable 1 V1 Type F VARIABLE MID RO E PR FIT F F F F 2 2 V2 F F 3 3 V3 F 4 A1 F 4 D1 F 5 A2 F 5 D2 F DESCRIPTION F 7 F 8 7 8 6 A3 F 6 D3 USRFAIL F F Material identification. A unique number or label not exceeding 8 characters must be specified. Mass density Young’s modulus LE.0: -E is load curve ID for Young’s modulus vs. plastic strain Poisson’s ratio Material parameter fit flag: EQ.0.0: Material parameters are used directly on card 3. EQ.1.0: Material parameters are determined from test data on cards 3 and 4 BETA Hardening parameter. Any value ranging from 0 (isotropic hardening) to 1 (kinematic hardening) may be input. *MAT_BARLAT_YLD2000 DESCRIPTION ITER Plastic iteration flag: EQ.0.0: Plane stress algorithm for stress return EQ.1.0: Secant iteration algorithm for stress return ITER provides an option of using three secant iterations for determining the thickness strain increment as experiments have shown that this leads to a more accurate prediction of shell thickness changes for rapid processes. A significant increase in computation time is incurred with this option so it should be used only for applications associated with high rates of loading and/or for implicit analysis. ISCALE Yield locus scaling flag: EQ.0.0: Scaling on – reference direction = rolling direction (default) EQ.1.0: Scaling off – reference direction arbitrary K Material parameter: HARD.EQ.1.0: 𝑘, strength coefficient for exponential hardening HARD.EQ.2.0: 𝑎 in Voce hardening law HARD.EQ.4.0: 𝑘, strength coefficient for Gosh hardening HARD.EQ.5.0: 𝑎 in Hocket-Sherby hardening law E0 Material parameter: HARD.EQ.1.0: 𝑒0, strain at yield for exponential hardening HARD.EQ.2.0: 𝑏 in Voce hardening law HARD.EQ.4.0: 𝜀0, strain at yield for Gosh hardening HARD.EQ.5.0: 𝑏 in Hocket-Sherby hardening law N Material parameter: HARD.EQ.1.0: 𝑛, exponent for exponential hardening HARD.EQ.2.0: 𝑐 in Voce hardening law HARD.EQ.4.0: 𝑛, exponent for Gosh hardening HARD.EQ.5.0: 𝑐 in Hocket-Sherby hardening law C Cowper-Symonds strain rate parameter, C, see formula below. VARIABLE DESCRIPTION P Cowper-Symonds strain rate parameter, 𝑝. 𝜎𝑦 𝑣(𝜀𝑝, 𝜀̇𝑝) = 𝜎𝑦(𝜀𝑝) ⎜⎛1 + [ ⎝ 𝜀̇𝑝 1/𝑝 ] ⎟⎞ ⎠ HARD Hardening law: EQ.1.0: Exponential hardening: 𝜎𝑦 = 𝑘(𝜀0 + 𝜀𝑝) EQ.2.0: Voce hardening: 𝜎𝑦 = 𝑎 − 𝑏𝑒−𝑐𝜀𝑝 EQ.3.0: Hansel hardening EQ.4.0: Gosh hardening: 𝜎𝑦 = 𝑘(𝜀0 + 𝜀𝑝) − 𝑝 EQ.5.0: Hocket-Sherby hardening: 𝜎𝑦 = 𝑎 − 𝑏𝑒−𝑐𝜀𝑝 LT.0.0: Absolute value defines load curve ID or table ID with yield stress as functions of plastic strain and in the lat- ter case also plastic strain rate. A CRCn CRAn Flow potential exponent. For face centered cubic (FCC) materials A = 8 is recommended and for body centered cubic (BCC) materials A = 6 may be used. Chaboche-Rousselier kinematic hardening parameters, see remarks. Chaboche-Rousselier kinematic hardening parameters, see remarks. ALPHA1 𝛼1, see equations below ⋮ ⋮ ALPHA8 𝛼8, see equations below SIG00 SIG45 SIG90 R00 R45 Yield stress in 00 direction Yield stress in 45 direction Yield stress in 90 direction 𝑅-value in 00 direction 𝑅-value in 45 direction *MAT_BARLAT_YLD2000 DESCRIPTION R90 𝑅-value in 90 direction SIGXX SIGYY SIGXY DXX DYY DXY CP T0 TREF TA0 A B C D P Q 𝑥𝑥-component of stress on yield surface . 𝑦𝑦-component of stress on yield surface . 𝑥𝑦-component of stress on yield surface . 𝑥𝑥-component of tangent to yield surface . 𝑦𝑦-component of tangent to yield surface . 𝑥𝑦-component of tangent to yield surface . Adiabatic temperature calculation option: EQ.0.0: Adiabatic temperature calculation is disabled. GT.0.0: CP is the specific heat 𝐶𝑝. Adiabatic temperature calculation is enabled. Initial temperature 𝑇0 of the material if adiabatic temperature calculation is enabled. Reference temperature for output of the yield stress as history variable. Reference temperature 𝑇𝐴0, the absolute zero for the used temperature scale, e.g. -273.15 if the Celsius scale is used and 0.0 if the Kelvin scale is used. Martensite rate equation parameter 𝐴, see equations below. Martensite rate equation parameter 𝐵, see equations below. Martensite rate equation parameter 𝐶, see equations below. Martensite rate equation parameter 𝐷, see equations below. Martensite rate equation parameter 𝑝, see equations below. Martensite rate equation parameter 𝑄, see equations below. E0MART Martensite rate equation parameter 𝐸0(mart) , see equations below. VARIABLE VM0 DESCRIPTION The initial volume fraction of martensite 0.0 < 𝑉𝑚0 < 1.0 may be initialised using two different methods: GT.0.0: 𝑉𝑚0 is set to VM0. LT.0.0: Can be used only when there are initial plastic strains εp present, e.g. when using *INITIAL_STRESS_- SHELL. The absolute value of VM0 is then the load curve ID for a function f that sets 𝑉𝑚0 = 𝑓 (𝜀𝑝). The function f must be a monotonically nondecreasing function of 𝜀𝑝. AHS BHS M N Hardening law parameter𝐴HS, see equations below. Hardening law parameter𝐵HS, see equations below. Hardening law parameter 𝑚, see equations below. Hardening law parameter 𝑛, see equations below. EPS0 Hardening law parameter 𝜀0, see equations below. HMART Hardening law parameter Δ𝐻𝛾→𝛼’, see equations below. K1 K2 Hardening law parameter 𝐾1, see equations below. Hardening law parameter 𝐾2, see equations below AOPT Material axes option: EQ.0.0: locally orthotropic with material axes determined by element nodes as shown in Figure M133-1. Nodes 1, 2, and 4 of an element are identical to the nodes used for the definition of a coordinate system as by *DEFINE_- COORDINATE_NODES EQ.2.0: globally orthotropic with material axes determined by vectors defined below, as with *DEFINE_COORDI- NATE_VECTOR EQ.3.0: locally orthotropic material axes determined by offsetting the material axes by an angle, OFFANG, from a line determined by taking the cross product of the vector v with the normal to the plane of the ele- ment. LT.0.0: the absolute value of AOPT is a coordinate system ID number (CID on *DEFINE_COORDINATE_NODES, *MAT_BARLAT_YLD2000 DESCRIPTION *DEFINE_COORDINATE_SYSTEM or *DEFINE_CO- ORDINATE_VECTOR). Available in R3 version of 971 and later. OFFANG Offset angle for AOPT = 3 P4 Material parameter: HARD.EQ.4.0: 𝑝 in Gosh hardening law HARD.EQ.5.0: 𝑞 in Hocket-Sherby hardening law HTFLAG Heat treatment flag : HTFLAG.EQ.0: Preforming stage HTFLAG.EQ.1: Heat treatment stage HTFLAG.EQ.2: Postforming stage HTA HTB HTC HTD Load curve/Table ID for postforming parameter A Load curve/Table ID for postforming parameter B Load curve/Table ID for postforming parameter C Load curve/Table ID for postforming parameter D A1, A2, A3 Components of vector 𝐚 for AOPT = 2 V1, V2, V3 Components of vector 𝐯 for AOPT = 3 D1, D2, D3 Components of vector 𝐝 for AOPT = 2 USRFAIL User defined failure flag EQ.0: no user subroutine is called EQ.1: user subroutine matusr_24 in dyn21.f is called Remarks: 1. Strain rate is accounted for using the Cowper and Symonds model which scales the yield stress with the factor 1 + ( 𝑝⁄ ) 𝜀̇ where 𝜀̇ is the strain rate. To ignore strain rate effects set both C and P to zero. 2. The yield condition for this material can be written 𝑓 (σ,α, 𝜀𝑝) = 𝜎eff(𝜎𝑥𝑥 − 2𝛼𝑥𝑥 − 𝛼𝑦𝑦, 𝜎𝑦𝑦 − 2𝛼𝑦𝑦 − 𝛼𝑥𝑥, 𝜎𝑥𝑦 − 𝛼𝑥𝑦) − 𝜎𝑌 𝑡 (𝜀𝑝, 𝜀̇𝑝, 𝛽) ≤ 0 where 𝜎eff(𝑠𝑥𝑥, 𝑠𝑦𝑦, 𝑠𝑥𝑦) = [ 1/𝑎 (𝜑′ + 𝜑′′)] 𝜑′ = ∣𝑋′1 − 𝑋′2∣𝑎 𝜑′′ = ∣2𝑋1 ′′ + X2 ′′∣𝑎 + ∣X1 ′′ + 2X2 ′′∣𝑎. The 𝑋′𝑖 and 𝑋′′𝑖 are eigenvalues of 𝑋′𝑖𝑗 and 𝑋′′𝑖𝑗 and are given by and ′ = 𝑋1 ′ = 𝑋2 ′′ = 𝑋1 ′′ = 𝑋2 (𝑋11 ′ + 𝑋22 ′ + √(𝑋11 ′ − 𝑋22 ′ )2 + 4𝑋12 ′ 2) (𝑋11 ′ + 𝑋22 ′ − √(𝑋11 ′ − 𝑋22 ′ )2 + 4𝑋12 ′ 2) (𝑋11 ′′ + 𝑋22 ′′ + √(𝑋11 ′′ − 𝑋22 ′′ )2 + 4𝑋12 ′′ 2) (𝑋11 ′′ + 𝑋22 ′′ − √(𝑋11 ′′ − 𝑋22 ′′ )2 + 4𝑋12 ′′ 2) respectively. The 𝑋′𝑖𝑗 and 𝑋′′𝑖𝑗 are given by ′ 𝑋11 ⎟⎟⎟⎞ ′ 𝑋22 ′ ⎠ 𝑋12 ′′ 𝑋11 ⎟⎟⎟⎞ ′′ 𝑋22 ′′ ⎠ 𝑋12 ⎜⎜⎜⎛ ⎝ ⎜⎜⎜⎛ ⎝ = = ′ 𝐿11 ′ 𝐿21 ⎜⎜⎜⎛ ⎝ ′′ 𝐿11 ′′ 𝐿21 ⎜⎜⎜⎛ ⎝ ′ 𝐿12 ′ 𝐿22 ′′ 𝐿12 ′′ 𝐿22 ⎟⎟⎟⎞ ′ ⎠ 𝐿33 ⎟⎟⎟⎞ ′′ ⎠ 𝐿33 𝑠𝑥𝑥 ⎟⎞ 𝑠𝑦𝑦 𝑠𝑥𝑦⎠ ⎜⎛ ⎝ 𝑠𝑥𝑥 ⎟⎞ 𝑠𝑦𝑦 𝑠𝑥𝑦⎠ ⎜⎛ ⎝ Where, ⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎞ ′ 𝐿11 ′ 𝐿12 ′ 𝐿21 ′ 𝐿22 ′ ⎠ 𝐿33 ′′ 𝐿11 ′′ 𝐿12 ′′ 𝐿21 ′′ 𝐿22 ′′ ⎠ 𝐿33 ⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎞ ⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎛ ⎝ ⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎛ ⎝ = −1 0 −1 ⎜⎜⎜⎜⎜⎜⎜⎛ ⎝ ⎟⎟⎟⎟⎟⎟⎟⎞ 3⎠ 𝛼1 ⎟⎞ 𝛼2 𝛼7⎠ ⎜⎛ ⎝ = ⎜⎜⎜⎜⎜⎜⎜⎛ ⎝ −2 1 −4 −4 4 −4 −4 8 −2 2 −2 −2 ⎟⎟⎟⎟⎟⎟⎟⎞ 9⎠ ⎟⎟⎟⎟⎟⎟⎟⎞ 𝛼3 𝛼4 𝛼5 𝛼6 𝛼8⎠ ⎜⎜⎜⎜⎜⎜⎜⎛ ⎝ The parameters 𝛼1 to 𝛼8 are the parameters that determines the shape of the yield surface. The material parameters can be determined from three uniaxial tests and a more general test. From the uniaxial tests the yield stress and R-values are used and from the general test an arbitrary point on the yield surface is used given by the stress components in the material system as 𝛔 = 𝜎𝑥𝑥 ⎟⎟⎞ 𝜎𝑦𝑦 𝜎𝑥𝑦⎠ ⎜⎜⎛ ⎝ together with a tangent of the yield surface in that particular point. For the latter the tangential direction should be determined so that 𝑑𝑥𝑥𝜀̇𝑥𝑥 𝑝 + 𝑑𝑦𝑦𝜀̇𝑦𝑦 𝑝 + 2𝑑𝑥𝑦𝜀̇𝑥𝑦 𝑝 = 0 The biaxial data can be set to zero in the input deck for LS-DYNA to just fit the uniaxial data. 3. A kinematic hardening model is implemented following the works of Chaboche and Roussilier. A back stress α is introduced such that the effective stress is computed as 𝜎eff = 𝜎eff(𝜎11 − 2𝛼11 − 𝛼22, 𝜎22 − 2𝛼22 − 𝛼11, 𝜎12 − 𝛼12) The back stress is the sum of up to four terms according to 𝛼𝑖𝑗 = ∑ 𝛼𝑖𝑗 𝑘=1 and the evolution of each back stress component is as follows 𝛿𝛼𝑖𝑗 𝑘 = 𝐶𝑘 (𝑎𝑘 𝑠𝑖𝑗 𝜎eff − 𝛼𝑖𝑗 𝑘 ) 𝛿𝜀𝑝 where 𝐶𝑘 and 𝑎𝑘 are material parameters, 𝑠𝑖𝑗 is the deviatoric stress tensor, 𝜎eff is the effective stress and 𝜀𝑝 is the effective plastic strain. The yield condition is for this case modified according to 𝑓 (𝛔, 𝛂, 𝜀𝑝) = 𝜎eff(𝜎𝑥𝑥 − 2𝛼𝑥𝑥 − 𝛼𝑦𝑦, 𝜎𝑦𝑦 − 2𝛼𝑦𝑦 − 𝛼𝑥𝑥, 𝜎𝑥𝑦 − 𝛼𝑥𝑦) − {𝜎𝑌 𝑡 (𝜀𝑝, 𝜀̇𝑝, 0) − ∑ 𝑎𝑘[1 − exp(−𝐶𝑘𝜀𝑝) ] } ≤ 0 𝑘=1 in order to get the expected stress strain response for uniaxial stress. 4. The Hansel hardening law is the same as in material 113 but is repeated here for the sake of convenience. The hardening is temperature dependent and therefore this material model must be run either in a coupled thermo-mechanical solution, using prescribed temperatures or using the adiabatic temperature calculation option. Setting the parameter CP to the specific heat Cp of the material activates the adiabatic tem- perature calculation that calculates the temperature rate from the equation 𝜎𝐢𝐣𝐷𝑖𝑗 𝜌𝐶𝑝 , 𝑇̇ = ∑ 𝑖,𝑗 where 𝛔: 𝐃𝑝 (the numerator) is the plastically dissipated heat. Using the Kelvin scale is recommended, even though other scales may be used without prob- lems. The hardening behaviour is described by the following equations. The marten- site rate equation is ∂𝑉𝑚 ∂𝜀̅𝑝 ⎧0 {{ ⎨ {{ ⎩ = 𝑉𝑚 𝑝 ( 1 − 𝑉𝑚 𝑉𝑚 ) 𝐵+1 𝐵 [1 − tanh(𝐶 + D × 𝑇)] 𝜀 < 𝐸0(mart) exp ( 𝑇 − 𝑇𝐴0 ) 𝜀̅𝑝 ≥ 𝐸0(mart) Where 𝜀̅𝑝 = effective plastic strain 𝑇 = temperature The martensite fraction is integrated from the above rate equation: 𝑉𝑚 = ∫ ∂𝑉𝑚 ∂𝜀̅𝑝 𝑑𝜀̅𝑝. It always holds that 0.0 < 𝑉𝑀 < 1.0. The initial martensite content is Vm0 and must be greater than zero and less than 1.0. Note that 𝑉𝑀0 is not used during a restart or when initializing the Vm history variable using *INITIAL_STRESS_- SHELL. The yield stress σy is 𝜎𝑦 = {𝐵𝐻𝑆 − (𝐵𝐻𝑆 − 𝐴𝐻𝑆)exp(−𝑚[𝜀̅𝑝 + 𝜀0]𝑛)}(𝐾1 + 𝐾2𝑇) + Δ𝐻𝛾→𝛼′𝑉𝑚. The parameters p and B should fulfill the following condition 1 + 𝐵 < 𝑝, if not fulfilled then the martensite rate will approach infinity as 𝑉𝑚 approaches zero. Setting the parameter 𝜀0 larger than zero, typical range 0.001-0.02 is rec- ommended. A part from the effective true strain a few additional history varia- bles are output, see below. History variables that are output for post-processing: Variable Description 24 Yield stress of material at temperature TREF. Useful to evaluate the strength of the material after e.g., a simulated forming operation. 25 Volume fraction martensite, Vm 26 CP.EQ.0.0: Not used CP.GT.0.0: Temperature from adiabatic temperature calculation. 5. Heat treatment for increasing the formability of prestrained aluminum sheets can be simulated through the use of HTFLAG, where the intention is to run a forming simulation in steps involving preforming, springback, heat treatment and postforming. In each step the history is transferred to the next via the use of dynain . The first two steps are per- formed with HTFLAG = 0 according to standard procedures, resulting in a 0corresponding to the prestrain. The heat treatment step is plastic strain field 𝜀𝑝 performed using HTFLAG = 1 in a coupled thermomechanical simulation, where the blank is heated. The coupling between thermal and mechanical is only that the maximum temperature 𝑇0 is stored as a history variable in the material model, this corresponding to the heat treatment temperature. Here it is important to export all history variables to the dynein file for the postforming step. In the final postforming step, HTFLAG = 2, the yield stress is then aug- mented by the Hocket-Sherby like term 0) Δ𝜎 = 𝑏 − (𝑏 − 𝑎)exp[−𝑐(𝜀𝑝 − 𝜀𝑝 ] where a, b, c and d are given as tables as functions of the heat treatment temper- ature 𝑇0 and prestrain 𝜀𝑝 0. That is, in the table definitions each load curve corre- sponds to a given prestrain and the load curve value is with respect to the heat treatment temperature, 𝑎 = 𝑎(𝑇0, 𝜀𝑝 𝑑 = 𝑑(𝑇0, 𝜀𝑝 𝑏 = 𝑏(𝑇0, 𝜀𝑝 𝑐 = 𝑐(𝑇0, 𝜀𝑝 0) 0), 0), 0), The effect of heat treatment is that the material strength decreases but harden- ing increases, thus typically, 𝑎 ≤ 0, 𝑏 ≥ 𝑎, 𝑐 > 0, 𝑑 > 0. *MAT_134 This is Material Type 134. The viscoelastic fabric model is a variation on the general viscoelastic model of material 76. This model is valid for 3 and 4 node membrane elements only and is strongly recommended for modeling isotropic viscoelastic fabrics where wrinkling may be a problem. For thin fabrics, buckling can result in an inability to support compressive stresses; thus, a flag is included for this option. If bending stresses are important use a shell formulation with model 76. Card 1 1 Variable MID Type I 2 RO F 3 4 5 6 BULK F 8 7 CSE F If fitting is done from a relaxation curve, specify fitting parameters on card 2, otherwise if constants are set on Viscoelastic Constant Cards LEAVE THIS CARD BLANK. Card 2 1 2 3 4 5 6 7 8 Variable LCID NT BSTART TRAMP LCIDK NTK BSTARTK TRAMPK Type F I F F F I F F Viscoelastic Constant Cards. Up to 6 cards may be input. A keyword card (with a “*” in column 1) terminates this input if less than 6 cards are used. These cards are not needed if relaxation data is defined. The number of terms for the shear behavior may differ from that for the bulk behavior: simply insert zero if a term is not included. Card 3 Variable Type 1 GI F 2 BETAI F 3 KI F 4 5 6 7 8 BETAKI F VARIABLE DESCRIPTION MID RO Material identification. A unique number must be specified. Mass density. BULK *MAT_VISCOELASTIC_FABRIC DESCRIPTION Elastic constant bulk modulus. is viscoelastic, then this modulus is used in determining the contact interface stiffness only. If the bulk behavior CSE Compressive stress flag (default = 0.0). EQ.0.0: don’t eliminate compressive stresses EQ.1.0: eliminate compressive stresses LCID NT BSTART Load curve ID if constants, Gi, and βi are determined via a least squares fit. This relaxation curve is shown below. Number of terms in shear fit. If zero the default is 6. Currently, the maximum number is set to 6. In the fit, β1 is set to zero, β2 is set to BSTART, β3 is 10 times β2, β4 is 10 times β3 , and so on. If zero, BSTART = 0.01. TRAMP Optional ramp time for loading. LCIDK Load curve ID for bulk behavior if constants, Ki, and βκi are determined via a least squares fit. This relaxation curve is shown below. NTK Number of terms desired in bulk fit. If zero the default is 6. Currently, the maximum number is set to 6. BSTARTK In the fit, βκ1 is set to zero, βκ2 is set to BSTARTK, βκ3 is 10 times βκ2, βκ4 If zero, BSTARTK = 0.01. is 10 times βκ3 , and so on. TRAMPK Optional ramp time for bulk loading. GI Optional shear relaxation modulus for the ith term BETAI Optional shear decay constant for the ith term KI Optional bulk relaxation modulus for the ith term BETAKI Optional bulk decay constant for the ith term Remarks: Rate effects are taken into accounted through linear viscoelasticity by a convolution integral of the form: 𝜎𝑖𝑗 = ∫ 𝑔𝑖𝑗𝑘𝑙 (𝑡 − 𝜏) ∂𝜀𝑘𝑙 ∂𝜏 𝑑𝜏 where 𝑔𝑖𝑗𝑘𝑙(𝑡 − 𝜏) is the relaxation function.If we wish to include only simple rate effects for the deviatoric stresses, the relaxation function is represented by six terms from the Prony series: 𝑔(𝑡) = ∑ 𝐺𝑚 𝑚=1 𝑒−𝛽𝑚 𝑡 We characterize this in the input by shear modulii, 𝐺𝑖, and decay constants, 𝛽𝑖. An arbitrary number of terms, up to 6, may be used when applying the viscoelastic model. For volumetric relaxation, the relaxation function is also represented by the Prony series in terms of bulk modulii: 𝑘(𝑡) = ∑ 𝐾𝑚 𝑚=1 𝑒−𝛽𝑘𝑚 𝑡 σ∕ε TRAMP 10n 10n+1 10n+2 10n+3 time optional ramp time for loading Figure M134-1. Stress Relaxation curve. For an example of a stress relaxation curve see Figure M134-1. This curve defines stress versus time where time is defined on a logarithmic scale. For best results, the points defined in the load curve should be equally spaced on the logarithmic scale. Furthermore, the load curve should be smooth and defined in the positive quadrant. If nonphysical values are determined by least squares fit, LS-DYNA will terminate with an error message after the initialization phase is completed. If the ramp time for loading is included, then the relaxation which occurs during the loading phase is taken into account. This effect may or may not be important. *MAT_135 This is material type 135. This anisotropic-viscoplastic material model adopts two yield criteria for metals with orthotropic anisotropy proposed by Barlat and Lian [1989] (Weak Texture Model) and Aretz [2004] (Strong Texture Model). 5 6 7 8 NUMFI EPSC WC TAUC Card 1 1 Variable MID Type A8 Card 2 1 2 RO F 2 3 E F 3 4 PR F 4 F 5 Variable SIGMA0 QR1 CR1 QR2 CR2 Type F F F F F YLD2003 Card. This card 3 format is used when FLG = 0. Card 3 Variable 1 A1 Type F 2 A2 F 3 A3 F 4 A4 F 5 A5 F F 6 K F 6 A6 F F 7 LC F 7 A7 F F 8 FLG F 8 A8 F Yield Surface Card. This card 3 format is used when FLG = 1. Card 3 1 2 3 4 5 6 7 8 Variable S00 S45 S90 SBB R00 R45 R90 RBB Type F F F F F F F YLD89 Card. This card 3 format used when FLG = 2. 5 6 7 8 Card 3 Variable Type 1 A F Card 4 1 2 C F 2 3 H F 3 4 P F 4 5 Variable QX1 CX1 QX2 CX2 EDOT 7 8 EMIN S100 F 7 F 8 7 8 7 8 6 M F 6 6 A3 F 6 D3 F F 3 3 ZP F 3 V3 F F 4 4 A1 F 4 D1 F F 5 5 A2 F 5 D2 F DESCRIPTION Material identification. A unique number or label not exceeding 8 characters must be specified. LS-DYNA R10.0 Type F Card 5 1 F 2 Variable AOPT BETA Type F F 2 YP F 2 V2 F Card 6 Variable 1 XP Type F Card 7 Variable 1 V1 Type F VARIABLE VARIABLE DESCRIPTION RO E PR NUMFI EPSC WC TAUC Mass density Young’s modulus Poisson’s ratio Number of through thickness integration points that must fail before the element is deleted (remember to change this number if switching between full and reduced integration type of elements). Critical value 𝜀𝑡𝐶 of the plastic thickness strain (used in the CTS fracture criterion). Critical value 𝑊𝑐 for the Cockcroft-Latham fracture criterion Critical value 𝜏𝑐 for the Bressan-Williams shear fracture criterion SIGMA0 Initial mean value of yield stress 𝜎0: GT.0.0: Constant value, LT.0.0: Load curve ID = -SIGMA0 which defines yield stress as a function of plastic strain. Hardening parameters QR1, CR1, QR2, and CR2 are ignored in that case. QR1 CR1 QR2 CR2 K LC A1 A2 A3 Isotropic hardening parameter 𝑄𝑅1 Isotropic hardening parameter 𝐶𝑅1 Isotropic hardening parameter 𝑄𝑅2 Isotropic hardening parameter 𝐶𝑅2 𝑘 equals half YLD2003 exponent 𝑚. Recommended value for FCC materials is 𝑚 = 8, i.e. 𝑘 = 4. First load curve number for process effects, i.e. the load curve describing the relation between the pre-strain and the yield stress 𝜎0. Similar curves for 𝑄𝑅1, 𝐶𝑅1, 𝑄𝑅2, 𝐶𝑅2, and 𝑊𝑐 must follow consecutively from this number. Yld2003 parameter 𝑎1 Yld2003 parameter 𝑎2 Yld2003 parameter 𝑎3 *MAT_WTM_STM DESCRIPTION A4 A5 A6 A7 A8 S00 S45 S90 SBB R00 R45 R90 RBB A C H P QX1 CX1 QX2 CX2 Yld2003 parameter 𝑎4 Yld2003 parameter 𝑎5 Yld2003 parameter 𝑎6 Yld2003 parameter 𝑎7 Yld2003 parameter 𝑎8 Yield stress in 0° direction Yield stress in 45° direction Yield stress in 90° direction Balanced biaxial flow stress R-ratio in 0° direction R-ratio in 45° direction R-ratio in 90° direction Balance biaxial flow ratio YLD89 parameter a YLD89 parameter c YLD89 parameter h YLD89 parameter p Kinematic hardening parameter 𝑄𝑥1 Kinematic hardening parameter 𝐶𝑥1 Kinematic hardening parameter 𝑄𝑥2 Kinematic hardening parameter 𝐶𝑥2 EDOT Strain rate parameter 𝜀̇0 M Strain rate parameter 𝑚 EMIN *MAT_135 DESCRIPTION Lower limit of the isotropic hardening rate 𝑑𝑅 𝑑𝜀̅. This feature is included to model a non-zero and linear/exponential isotropic work hardening rate at large values of effective plastic strain. If the isotropic work hardening rate predicted by the utilized Voce- type work hardening rule falls below the specified value it is substituted by the prescribed value or switched to a power-law hardening if S100.NE.0. This option should be considered for problems involving extensive plastic deformations. If process dependent material characteristics are prescribed, i.e. if LC .GT. 0 the same minimum tangent modulus is assumed for all the prescribed work hardening curves. If instead EMIN.LT.0 then – EMIN defines the plastic strain value at which the linear or power-law hardening approximation commences. S100 AOPT Yield stress at 100% strain for using a power-law approximation beyond the strain defined by EMIN. Material axes option : EQ.0.0: locally orthotropic with material axes determined by element nodes 1, 2, and 4, as with *DEFINE_COORDI- NATE_NODES, and then rotated about the shell ele- ment normal by an angle BETA. EQ.2.0: globally orthotropic with material axes determined by vectors defined below, as with *DEFINE_COORDI- NATE_VECTOR. EQ.3.0: locally orthotropic material axes determined by rotating the material axes about the element normal by an angle, BETA, from a line in the plane of the element defined by the cross product of the vector v with the element normal. LT.0.0: the absolute value of AOPT is a coordinate system ID number (CID on *DEFINE_COORDINATE_NODES, *DEFINE_COORDINATE_SYSTEM or *DEFINE_CO- ORDINATE_VECTOR). Available in R3 version of 971 and later.. BETA Material angle in degrees for AOPT = 0 or 3, may be overwritten on the element card, see *ELEMENT_SHELL_BETA. XP YP ZP Coordinates of point p for AOPT = 1. *MAT_WTM_STM DESCRIPTION A1 A2 A3 Components of vector a for AOPT = 2. V1 V2 V3 Components of vector v for AOPT = 3 D1 D2 D3 Components of vector d for AOPT = 2. Remarks: If FLG = 1, i.e. if the yield surface parameters 𝑎1−𝑎8 are identified on the basis of prescribed material data internally in the material routine, files with point data for plotting of the identified yield surface, along with the predicted directional variation of the yield stress and plastic flow are generated in the directory where the LS-DYNA analysis is run. Four different files are generated for each specified material. These files are named according to the scheme: 1. Contour_1# 2. Contour_2# 3. Contour_3# 4. R_and_S# Where # is a value starting at 1. The three first files contain contour data for plotting of the yield surface as shown in Figure M135-2. To generate these plots a suitable plotting program should be adopted and for each file/plot, column A should be plotted vs. columns B. For a more detailed description of these plots it is referred to References. Figure M135-3 further shows a plot generated from the final file named ‘R_and_S#’ showing the directional dependency of the normalized yield stress (column A vs. B) and plastic strain ratio (column B vs. C). The yield condition for this material can be written 𝑡(σ, α, 𝜀𝑝, 𝜀̇𝑝) = 𝜎eff(σ, α) − 𝜎𝑌(𝜀𝑝, 𝜀̇𝑝) where 𝜎𝑌 = [𝜎0 + 𝑅(𝜀𝑝)] (1 + ) 𝜀̇𝑝 𝜀̇0 where the isotropic hardening reads 𝑅(𝜀̇𝑝) = 𝑄𝑅1[1 − exp(−𝐶𝑅1𝜀𝑝)] + 𝑄𝑅2[1 − exp(−𝐶𝑅2𝜀𝑝)]. For the Weak Texture Model the yield function is defined as 𝜎eff = [ {𝑎(𝑘1 + 𝑘2)𝑚 + 𝑎(𝑘1 − 𝑘2)𝑚 + 𝐶(2𝑘2)𝑚}] where 𝑘1 = 𝜎𝑥 + ℎ 𝜎𝑦 √ √√ ⎷ ( 𝜎𝑥 + ℎ 𝜎𝑦 ) 𝑘2 = + (𝑟 𝜎𝑥𝑦) . For the Strong Texture Model the yield function is defined as 𝜎eff = { where [(𝜎+ ′ )𝑚 + (𝜎− ′ )𝑚 + (𝜎+ ′′ − 𝜎− ′′)𝑚]} ′ = σ± 𝑎8𝜎𝑥 + 𝑎1𝜎𝑦 ± √( 𝑎2𝜎𝑥 − 𝑎3𝜎𝑦 ) + 𝑎4 2𝜎𝑥𝑦 2 ′′ = σ± 𝜎𝑥 + 𝜎𝑦 ± √( 𝑎5𝜎𝑥 − 𝑎6𝜎𝑦 ) + 𝑎7 2 𝜎𝑥𝑦. Kinematic hardening can be included by α = ∑ α𝑅 𝑅=1 where each of the kinematic hardening variables 𝛼𝑅 is independent and obeys a nonlinear evolutionary equation in the form where the effective stress 𝜎̅̅̅̅̅ is defined as α̇𝑅 = 𝐶𝛼𝑖 (𝑄𝛼𝑖 − α𝑅) 𝜀̇𝑝 where 𝜎̅̅̅̅̅ = 𝜎eff(τ) τ = σ − α. Critical thickness strain failure in a layer is assumed to occur when 𝜀𝑡 ≤ 𝜀𝑡𝑐 where 𝜀𝑡𝑐 is a material parameter. It should be noted that 𝜀𝑡𝑐 is a negative number (i.e. failure is assumed to occur only in the case of thinning). Cockcraft and Latham fracture is assumed to occur when where 𝜎1 is the maximum principal stress and 𝑊𝐶 is a material parameter. 𝑊 = ∫ max(𝜎1, 0)𝑑𝜀𝑝 ≥ 𝑊𝐶 History Variable 1 2 3 4 5 6 7 8 9 10 11 12 13 14 Description Isotropic hardening value 𝑅1 Isotropic hardening value 𝑅2 Increment in effective plastic strain Δ𝜀̅ Not defined, for internal use in the material model Not defined, for internal use in the material model Not defined, for internal use in the material model Failure in integration point EQ.0: No failure EQ.1: Failure due to EPSC, i.e. 𝜀𝑡 ≥ 𝜀𝑡𝑐. EQ.2: Failure due to WC, i.e. 𝑊 ≥ 𝑊𝑐. EQ.3: Failure due to TAUC, i.e. 𝜏 ≥ 𝜏𝑐 Sum of incremental strain 𝜀𝑥𝑥 = ∑ Δ𝜀𝑥𝑥 Sum of 𝜀𝑦𝑦 = ∑ Δ𝜀𝑦𝑦 incremental strain in in local element x-direction: local element y-direction: Value of theh Cockcroft-Latham failure parameter 𝑊 = ∑ 𝜎1Δ𝑝 Plastic strain component in thickness direction 𝜀𝑡 Mean value of increments in plastic strain through the thickness (For use with the non-local instability criterion. Note that constant lamella thickness is assumed and the instability criterion can give unrealistic results if used with a user-defined integration rule with varying lamella thickness.) Not defined, for internal use in the material model Nonlocal value 𝜌 = Δ𝜀3 Ω Δ𝜀3 Table M135-1. 1.5 0.5 -0.5 -1 -1.5 -1.5 -1 -0.5 1.5 0.75 xy -0.75 -1.5 0.5 1.5 -1.5 -0.75 (A) 1.5 0.75 xy -0.75 -1.5 0.75 1.5 √2(σ x+σ 2σ y) (B) 0.75 1.5 -1.5 -0.75 √2(σ x-σ 2σ y) (C) Figure M135-2. Contour plots of the yield surface generated from the files (a) ‘Contour_1<#>’, (b) Contour_2<#>’, and (c) ‘Contour_3<#>’. 1.1 1.05 σα 0.95 1.6 1.2 0.8 0.4 Rα 0.9 30 α [deg] 60 90 Figure M135-3. Predicted directional variation of the yield stress and plastic flow generated from the file ‘R_and_S<#>’. *MAT_135_PLC This is Material Type 135. This anisotropic material adopts the yield criteria proposed by Aretz [2004]. The material strength is defined by McCormick’s constitutive relation for materials exhibiting negative steady-state Strain Rate Sensitivity (SRS). McCormick [1998] and Zhang, McCormick and Estrin [2001]. 5 6 7 8 NUMFI EPSC WC TAUC Card 1 1 Variable MID Type A8 Card 2 1 2 RO F 2 3 E F 3 4 PR F 4 F 5 Variable SIGMA0 QR1 CR1 QR2 CR2 Type F F F F F Card 3 Variable 1 A1 Type F Card 4 Variable Type 1 S F 2 A2 F 2 H F 3 A3 F 3 4 A4 F 4 5 A5 F 5 OMEGA TD ALPHA EPS0 F F F F F 6 K F 6 A6 F 6 F 7 7 A7 F 7 F 8 8 A8 F Card 5 1 2 3 4 5 6 7 8 Variable AOPT BETA Type F F Card 6 Variable 1 XP Type F Card 7 Variable 1 V1 Type F 2 YP F 2 V2 F 3 ZP F 3 V3 F 4 A1 F 4 D1 F 5 A2 F 5 D2 F 6 A3 F 6 D3 F 7 8 7 8 VARIABLE DESCRIPTION MID RO E PR NUMFI EPSC WC TAUC Material identification. A unique number or label not exceeding 8 characters must be specified. Mass density Young’s modulus Poisson’s ratio Number of through thickness integration points that must fail before the element is deleted (remember to change this number if switching between full and reduced integration type of elements). Critical value 𝜀𝑡𝐶 of the plastic thickness strain. Critical value 𝑊𝑐 for the Cockcroft-Latham fracture criterion. Critical value 𝜏𝑐 for the shear fracture criterion. SIGMA0 Initial yield stress 𝜎0 VARIABLE DESCRIPTION QR1 CR1 QR2 CR2 K A1 A2 A3 A4 A5 A6 A7 A8 S H Isotropic hardening parameter, 𝑄𝑅1 Isotropic hardening parameter, 𝐶𝑅1 Isotropic hardening parameter, 𝑄𝑅2 Isotropic hardening parameter, 𝐶𝑅2 k equals half the exponent m for the yield criterion Yld2003 parameter, 𝑎1 Yld2003 parameter, 𝑎2 Yld2003 parameter, 𝑎3 Yld2003 parameter, 𝑎4 Yld2003 parameter, 𝑎5 Yld2003 parameter, 𝑎6 Yld2003 parameter, 𝑎7 Yld2003 parameter, 𝑎8 Dynamic strain aging parameter, S. Dynamic strain aging parameter, H. OMEGA Dynamic strain aging parameter, Ω. TD Dynamic strain aging parameter, 𝑡𝑑. ALPHA Dynamic strain aging parameter, 𝛼. EPS0 AOPT Dynamic strain aging parameter, 𝜀̇0. Material axes option EQ.0.0: Locally orthotropic with material axes determined by element nodes as shown in Figure M2-1, and then ro- tated about the shell element normal by the angle BE- TA. Nodes 1, 2 and 4 of an element are identical to the nodes used for the definition of a coordinate system as by *DEFINE_COORDINATE_NODES. VARIABLE DESCRIPTION EQ.2.0: Globally orthotropic with material axes determined by vectors defined below, as with *DEFINE_COORDI- NATE_VECTOR. EQ.3.0: Locally orthotropic material axes determined by offsetting the material axes by an angle, BETA, from a line determined by taking the cross product of the vec- tor v with the normal to the plane of the element. LT.0.0: the absolute value of AOPT is a coordinate system ID number (CID on *DEFINE_COORDINATE_NODES, *DEFINE_COORDINATE_SYSTEM or *DEFINE_CO- ORDINATE_VECTOR). Available in R3 version of 971 and later. BETA Material angle in degrees for AOPT = 0 and 3, may be overwritten on the element card, see *ELEMENT_SHELL_BETA. XP, YP, ZP Coordinates of point p for AOPT = 1. A1, A2, A3 Components of vector a for AOPT = 2. V1, V2, V3 Components of vector v for AOPT = 3. D1, D2, D3 Components of vector d for AOPT = 2. Remarks: The yield function is defined as 𝑓 = 𝑓 ̅(σ) − [𝜎𝑌(𝑡𝑎) + 𝑅(𝜀𝑝) + 𝜎𝑣(𝜀̇𝑝)] where the equivalent stress 𝜎eq is defined as by an anisotropic yield criterion 𝜎eq = [ (∣𝜎′1∣𝑚 + ∣𝜎′2∣𝑚 + ∣𝜎′′1 − 𝜎′′2∣)] where and { 𝜎′1 𝜎′2 } = 𝑎8𝜎𝑥𝑥 + 𝑎1𝜎𝑦𝑦 ± √( 𝑎2𝜎𝑥𝑥 − 𝑎3𝜎𝑦𝑦 ) + 𝑎4 2𝜎𝑥𝑦 2 𝜎′′1 { 𝜎′′2 } = 𝜎𝑥𝑥 + 𝜎𝑦𝑦 ± √( 𝑎5𝜎𝑥𝑥 − 𝑎6𝜎𝑦𝑦 ) + 𝑎7 2𝜎𝑥𝑦 The strain hardening function R is defined by the extended Voce law 𝑅(𝜀𝑝) = ∑ 𝑄𝑅𝑖(1 − exp(−𝐶𝑅𝑖𝜀𝑝)) 𝑖=1 where 𝜀𝑝 is the effective (or accumulated) plastic strain, and 𝑄𝑅𝑖and 𝐶𝑅𝑖 are strain hardening parameters. Viscous stress 𝜎𝑣 is given by 𝜎𝑣 = (𝜀̇𝑝) = 𝑠 ln (1 + 𝜀̇𝑝 𝜀̇0 ) where S represents the instantaneous strain rate sensitivity (SRS) and 𝜀̇0 is a reference strain rate. In this model the yield strength, including the contribution from dynamic strain aging (DSA) is defined as 𝜎𝑌(𝑡𝑎) = 𝜎0 + SH [1 − exp {− ( ) 𝑡𝑎 𝑡𝑑 }] where 𝜎0is the yield strength for vanishing average waiting time, 𝑡𝑎, i.e. at high strain rates, and H, 𝛼and 𝑡𝑑 are material constants linked to dynamic strain aging. It is noteworthy that 𝜎𝑌 is an increasing function of 𝑡𝑎. The average waiting time is defined by the evolution equation 𝑡 ̇𝑎 = 1 − 𝑡𝑎 𝑡𝑎,𝑠𝑠 where the quasi-steady waiting time 𝑡𝑎,𝑠𝑠 is given as 𝑡𝑎,𝑠𝑠 = 𝜀̇𝑝 where Ω is the strain produced by all mobile dislocations moving to the next obstacle on their path. *MAT_CORUS_VEGTER This is Material Type 136, a plane stress orthotropic material model for metal forming. Yield surface construction is based on the interpolation by second-order Bezier curves, and model parameters are determined directly from a set of mechanical tests conducted for a number of directions. For each direction, four mechanical tests are carried out: a uniaxial, an equi-biaxial, a plane strain tensile test and a shear test. These test results are used to determine the coefficients of the Fourier directional dependency field. For a more detailed description please see Vegter and Boogaard [2006]. Card 1 1 Variable MID Type A8 Card 2 1 2 RO F 2 3 E F 3 4 PR F 4 5 N F 5 Variable SYS SIP SHS SHL ESH Type F Card 3 1 Variable AOPT Type Card 4 Variable 1 XP Type F F 2 2 YP F F 3 3 ZP F F 4 4 A1 F F 5 5 A2 F 6 FBI F 6 E0 F 6 6 A3 F 7 8 RBI0 LCID F 7 F 8 ALPHA LCID2 F 7 F 8 7 Variable 1 V1 Type F 2 V2 F 3 V3 F 4 D1 F 5 D2 F 6 D3 F *MAT_136 7 8 BETA F Experimental Data Cards. The next N cards contain experimental data obtained from four mechanical tests for a group of equidistantly placed directions 𝜃𝑖 = 𝑖𝜋 2𝑁 , 𝑖 = 0, 1, 2, … , 𝑁. Card 6 1 2 3 4 5 6 7 8 Variable FUN-I RUN-I FPS1-I FPS2-I FSH-I Type F F F F F VARIABLE DESCRIPTION MID RO E PR N FBI RBI0 LCID Material identification. A unique number or label not exceeding 8 characters must be specified. Material density Elastic Young’s modulus Poisson’s ratio |N| is order of Fourier series (i.e., number of test groups minus one). The minimum number for |N| is 2, and the maximum is 12. GE.0.0: Explicit cutting-plane return mapping algorithm LT.0.0: Fully implicit return mapping algorithm (more robust) Normalized yield stress 𝜎𝑏𝑖 for equi-biaxial test. Strain ratio 𝜌𝑏𝑖(0°) = 𝜀̇2(0°)/𝜀̇1(0°) for equi-biaxial test in the rolling direction. Stress-strain curve ID. If defined, SYS, SIP, SHS, SHL, ESH, and E0 are ignored. SYS Static yield stress, 𝜎0. SIP SHS SHL ESH E0 ALPHA LCID2 *MAT_CORUS_VEGTER DESCRIPTION Stress increment parameter, Δ𝜎𝑚. Strain hardening parameter for small strain, 𝛽. Strain hardening parameter for larger strain, Ω. Exponent for strain hardening, n. Initial plastic strain, 𝜀0 𝛼 distribution of hardening used in the curve-fitting. 𝛼 = 0 pure kinematic hardening and 𝛼 = 1 provides pure isotropic hardening. Curve ID. The curve defines Young’s modulus scaling factor with respect to the plastic strain. By default it is assumed that Young’s modulus remains constant. Effective value is between 0 and 1. AOPT Material axes option : EQ.0.0: locally orthotropic with material axes determined by element nodes 1, 2, and 4, as with *DEFINE_COORDI- NATE_NODES, and then rotated about the shell ele- ment normal by the angle BETA. EQ.2.0: globally orthotropic with material axes determined by vectors defined below, as with *DEFINE_COORDI- NATE_VECTOR. EQ.3.0: locally orthotropic material axes determined by rotating the material axes about the element normal by an angle, BETA, from a line in the plane of the element defined by the cross product of the vector v with the element normal. LT.0.0: the absolute value of AOPT is a coordinate system ID number (CID on *DEFINE_COORDINATE_NODES, *DEFINE_COORDINATE_SYSTEM or *DEFINE_CO- ORDINATE_VECTOR). XP, YP, ZP Coordinates of point p for AOPT = 1. A1, A2, A3 Components of vector a for AOPT = 2. V1, V2, V3 Components of vector v for AOPT = 3 Figure M136-1. Bézier interpolation curve. VARIABLE DESCRIPTION D1, D2, D3 Components of vector d for AOPT = 2. Material angle in degrees for AOPT = 0 and 3, may be overwritten on the element card, see *ELEMENT_SHELL_BETA. Normalized yield stress 𝜎un for uniaxial test for the ith direction. Strain ratio (R-value) for uniaxial test for the ith direction. First normalized yield stress 𝜎ps1 for plain strain test for the ith direction. Second normalized yield stress 𝜎ps2 for plain strain test for the ith direction. First normalized yield stress 𝜎sh for pure shear test for the ith direction. BETA FUN-I RUN-I FPS1-I FPS2-I FSH-I Remarks: The Vegter yield locus is section-wise defined by quadratic Bézier interpolation functions. Each individual curve uses 2 reference points and a hinge point in the principal plane stress space, see Figure M136-1. The mathematical description of the Bézier interpolation is given by: Figure M136-2. Vegter yield surface. 𝜎1 ( 𝜎2 ) = ( 𝜎1 𝜎2 ) + 2𝜇 [( 𝜎1 𝜎2 − ( 𝜎1 𝜎2 ) ) ] + 𝜇2 [( 𝜎1 𝜎2 + ( 𝜎1 𝜎2 ) − 2( ) 𝜎1 𝜎2 ] ) where (𝜎1, 𝜎2)0 is the first reference point, (𝜎1, 𝜎2)1 is the hinge point, and (𝜎1, 𝜎2)2 is the second reference point. 𝜇 is a parameter which determines the location on the curve (0 ≤ 𝜇 ≤ 1). Four characteristic stress states are selected as reference points: the equi-biaxial point (𝜎𝑏𝑖, 𝜎𝑏𝑖), the plane strain point (𝜎𝑝𝑠1, 𝜎𝑝𝑠2), the uniaxial point (𝜎𝑢𝑛, 0) and the pure shear point (𝜎𝑠ℎ, −𝜎𝑠ℎ), see Figure M136-2. Between the 4 stress points, 3 Bézier curves are used to interpolate the yield locus. Symmetry conditions are used to construct the complete surface. The yield locus in Figure M136-2 shows the reference points of experiments for one specific direction. The reference points can also be determined for other angles to the rolling direction (planar angle 𝜃). E.g. if N = 2 is chosen, normalized yield stresses for directions 0°, 45°, and 90° should be defined. A Fourier series is used to interpolate intermediate angles between the measured points. The Vegter yield function with isotropic hardening (ALPHA = 1) is given as: 𝜙 = 𝜎𝑒𝑞(𝜎1, 𝜎2, 𝜃) − 𝜎𝑦(𝜀̅𝑝) with the equivalent stress 𝜎𝑒𝑞 obtained from the appropriate Bézier function related to the current stress state. The uni-axial yield stress 𝜎𝑦 can be defined as stress-strain curve LCID or alternatively as a functional expression: 𝜎𝑦 = 𝜎0 + Δ𝜎𝑚[𝛽(𝜀̅𝑝 + 𝜀0) + (1 − 𝑒−Ω(𝜀̅𝑝+𝜀0)) ] In case of kinematic hardening (ALPHA < 1), the standard stress tensor is replaced by a relative stress tensor, defined as the difference between the stress tensor and a back stress tensor. To determine the yield stress or reference points of the Vegter yield locus, four mechanical tests have to be performed for different directions. A good description about the material characterization procedure can be found in Vegter et al. (2003). *MAT_COHESIVE_MIXED_MODE This is Material Type 138. This model is a simplification of *MAT_COHESIVE_GENER- AL restricted to linear softening. It includes a bilinear traction-separation law with quadratic mixed mode delamination criterion and a damage formulation. This material model can be used only with cohesive element fomulations; see the variable ELFORM in *SECTION_SOLID and *SECTION_SHELL. 6 ET F 6 7 8 GIC GIIC F 7 F 8 Card 1 1 2 3 4 5 Variable MID RO ROFLG INTFAIL EN Type A8 Card 2 1 Variable XMU Type F VARIABLE MID F 2 T F F 3 S F F 4 F 5 UND UTD GAMMA F F F DESCRIPTION Material identification. A unique number or label not exceeding 8 characters must be specified. RO Mass density ROFLG INTFAIL EN ET Flag for whether density is specified per unit area or volume. ROFLG = 0 specified density per unit volume (default), and ROFLG = 1 specifies the density is per unit area for controlling the mass of cohesive elements with an initial volume of zero. The number of integration points required for the cohesive element to be deleted. If it is zero, the element will not be deleted even if it satisfies the failure criterion. The value of INTFAIL may range from 1 to 4, with 1 the recommended value. The stiffness (units of stress / length) normal to the plane of the cohesive element. The stiffness (units of stress / length) in the plane of the cohesive element. VARIABLE DESCRIPTION GIC GIIC XMU T S UND UTD Energy release rate for mode I (units of stress × length) Energy release rate for mode II (units of stress × length) Exponent of the mixed mode criteria Peak traction (stress units) in normal direction LT.0.0: Load curve ID = (-T) which defines peak traction in normal direction as a function of element size. See re- marks. Peak traction (stress units) in tangential direction LT.0.0: Load curve ID = (-S) which defines peak traction in tangential direction as a function of element size. See remarks. Ultimate displacement in the normal direction Ultimate displacement in the tangential direction GAMMA Additional exponent for Benzeggagh-Kenane law (default = 1.0) Remarks: The ultimate displacements in the normal and tangential directions are the displacements at the time when the material has failed completely, i.e., the tractions are zero. The linear stiffness for loading followed by the linear softening during the damage provides an especially simple relationship between the energy release rates, the peak tractions, and the ultimate displacements: GIC = T × GIIC = S × UND UTD If the peak tractions aren’t specified, they are computed from the ultimate displace- ments. See Fiolka and Matzenmiller [2005] and Gerlach, Fiolka and Matzenmiller [2005]. In this cohesive material model, the total mixed-mode relative displacement 𝛿𝑚 is 2 , where 𝛿𝐼 = 𝛿3 is the separation in normal direction (mode I) defined as 𝛿𝑚 = √𝛿𝐼 2 + 𝛿𝐼𝐼 3 2 1 II traction 0δ II II Fδ Figure M138-1. Mixed-mode traction-separation law and 𝛿𝐼𝐼 = √𝛿1 damage initiation displacement 𝛿0 (onset of softening) is given by 2 is the separation in tangential direction (mode II). The mixed-mode 2 + 𝛿2 𝛿0 = 𝛿𝐼 0𝛿𝐼𝐼 0 √ 1 + 𝛽2 0 )2 + (𝛽𝛿𝐼 (𝛿𝐼𝐼 0)2 0 = 𝑇/EN and 𝛿𝐼𝐼 0 = 𝑆/ET are the single mode damage inititation separations where 𝛿𝐼 and 𝛽 = 𝛿𝐼𝐼/𝛿𝐼 is the “mode mixity” . The ultimate mixed-mode displacement 𝛿𝐹 (total failure) for the power law (XMU > 0) is: ⎡( ⎢ ⎣ and alternatively for the Benzeggagh-Kenane law [1996] (XMU < 0): 𝛿𝐹 = + ( ) ) 2(1 + 𝛽2) 𝛿0 ET × 𝛽2 GIIC EN GIC XMU XMU XMU − 1 ⎤ ⎥ ⎦ 𝛿𝐹 = 𝛿0 ( 1 1 + 𝛽2 EN𝛾 + 1/𝛾 𝛽2 1 + 𝛽2 ET𝛾) ⎡GIC + (GIIC − GIC) ( ⎢ ⎣ 𝛽2 × ET EN + 𝛽2 × ET ) |XMU| ⎤ ⎥ ⎦ A reasonable choice for the exponent 𝛾 would be GAMMA = 1.0 (default) or GAMMA = 2.0. In this model, damage of the interface is considered, i.e. irreversible conditions are enforced with loading/unloading paths coming from/pointing to the origin. Peak tractions 𝑇 and/or 𝑆 can be defined as functions of characteristic element length (square root of midsurface area) via load curve. This option is useful to get nearly the same global responses (e.g. load-displacement curve) with coarse meshes when compared to a fine mesh solution. In general, lower peak traction values are needed for coarser meshes QMAX GC Displacement Figure M138-2. Bilinear traction-separation Two error checks have been implemented for this material model in order to ensure proper material data. Since the traction versus displacement curve is fairly simple (triangular shaped), equations can be developed to ensure that the displacement, 𝐿, at the peak load (QMAX), is smaller than the ultimate distance for failure, 𝑢. See Figure M138-2 for the used notation. One has that And, GC = 𝑢 × QMAX 𝐿 = QMAX . To ensure that the peak is not past the failure point, 𝑢 𝐿 must be larger than 1. 2GC EL where GC is the energy release rate. This gives 𝑢 = , = 2GC EL × 𝐿 = 2GC 𝐸 ( QMAX 2 > 1. ) The error checks are then done for tension and pure shear, respectively, = (2GIC) EN( 𝑇 EN 2 > 1, ) = (2GIIC) ET ( 𝑆 ET ) 2 > 1. *MAT_MODIFIED_FORCE_LIMITED This is Material Type 139. This material for the Belytschko-Schwer resultant beam is an extension of material 29. In addition to the original plastic hinge and collapse mechanisms of material 29, yield moments may be defined as a function of axial force. After a hinge forms, the moment transmitted by the hinge is limited by a moment- plastic rotation relationship. Card 1 1 Variable MID 2 RO Type A8 F 3 E F 4 PR F 5 DF F 6 7 8 AOPT YTFLAG ASOFT F F F Default none none none none 0.0 0.0 0.0 0.0 Card 2 1 Variable M1 Type F Default none Card 3 1 2 M2 F 0 2 3 M3 F 0 3 4 M4 F 0 4 5 M5 F 0 5 6 M6 F 0 6 7 M7 F 0 7 8 M8 F 0 8 Variable LC1 LC2 LC3 LC4 LC5 LC6 LC7 LC8 Type F Default none F 0 F 0 F 0 F 0 F 0 F 0 F Card 4 1 2 3 4 5 6 7 8 Variable LPS1 SFS1 LPS2 SFS2 YMS1 YMS2 Type Default F 0 F F F F F 1.0 LPS1 1.0 1.0E+20 YMS1 Card 5 1 2 3 4 5 6 7 8 Variable LPT1 SFT1 LPT2 SFT2 YMT1 YMT2 Type Default F 0 F F F F F 1.0 LPT1 1.0 1.0E+20 YMT1 Card 6 1 2 3 4 5 6 7 8 Variable LPR SFR YMR Type Default F 0 F F 1.0 1.0E+20 Card 7 1 2 3 4 5 6 7 8 Variable LYS1 SYS1 LYS2 SYS2 LYT1 SYT1 LYT2 SYT2 Type Default F 0 F 1.0 F 0 F 1.0 F 0 F 1.0 F 0 F 1.0 Card 8 1 2 3 4 5 6 7 8 Variable LYR SYR Type Default F 0 F 1.0 Card 9 1 2 3 4 5 6 7 8 Variable HMS1_1 HMS1_2 HMS1_3 HMS1_4 HMS1_5 HMS1_6 HMS1_7 HMS1_8 Type Default F 0 Card 10 1 F 0 2 F 0 3 F 0 4 F 0 5 F 0 6 F 0 7 F 0 8 Variable LPMS1_1 LPMS1_2 LPMS1_3 LPMS1_4 LPMS1_5 LPMS1_6 LPMS1_7 LPMS1_8 Type Default F 0 Card 11 1 F 0 2 F 0 3 F 0 4 F 0 5 F 0 6 F 0 7 F 0 8 Variable HMS2_1 HMS2_2 HMS2_3 HMS2_4 HMS2_5 HMS2_6 HMS2_7 HMS2_8 Type Default F 0 F 0 F 0 F 0 F 0 F 0 F 0 F Card 12 1 2 3 4 5 6 7 8 Variable LPMS2_1 LPMS2_2 LPMS2_3 LPMS2_4 LPMS2_5 LPMS2_6 LPMS2_7 LPMS2_8 Type Default F 0 Card 13 1 F 0 2 F 0 3 F 0 4 F 0 5 F 0 6 F 0 7 F 0 8 Variable HMT1_1 HMT1_2 HMT1_3 HMT1_4 HMT1_5 HMT1_6 HMT1_7 HMT1_8 Type Default F 0 Card 14 1 F 0 2 F 0 3 F 0 4 F 0 5 F 0 6 F 0 7 F 0 8 Variable LPMT1_1 LPMT1_2 LPMT1_3 LPMT1_4 LPMT1_5 LPMT1_6 LPMT1_7 LPMT1_8 Type Default F 0 Card 15 1 F 0 2 F 0 3 F 0 4 F 0 5 F 0 6 F 0 7 F 0 8 Variable HMT2_1 HMT2_2 HMT2_3 HMT2_4 HMT2_5 HMT2_6 HMT2_7 HMT2_8 Type Default F 0 F 0 F 0 F 0 F 0 F 0 F 0 F Card 16 1 2 3 4 5 6 7 8 Variable LPMT2_1 LPMT2_2 LPMT2_3 LPMT2_4 LPMT2_5 LPMT2_6 LPMT2_7 LPMT2_8 Type Default F 0 Card 17 1 F 0 2 F 0 3 F 0 4 F 0 5 F 0 6 F 0 7 F 0 8 Variable HMR_1 HMR_2 HMR_3 HMR_4 HMR_5 HMR_6 HMR_7 HMR_8 Type Default F 0 Card 18 1 F 0 2 F 0 3 F 0 4 F 0 5 F 0 6 F 0 7 F 0 8 Variable LPMR_1 LPMR_2 LPMR_3 LPMR_4 LPMR_5 LPMR_6 LPMR_7 LPMR_8 Type Default F 0 F 0 F 0 F 0 F 0 F 0 F 0 F 0 VARIABLE DESCRIPTION MID RO E PR DF Material identification. A unique number or label not exceeding 8 characters must be specified. Mass density Young’s modulus Poisson’s ratio Damping factor, see definition in notes below. A proper control for the timestep has to be maintained by the user! *MAT_MODIFIED_FORCE_LIMITED DESCRIPTION AOPT Axial load curve option: EQ.0.0: axial load curves are force versus strain, EQ.1.0: axial load curves are force versus change in length. LT.0.0: the absolute value of AOPT is a coordinate system ID number (CID on *DEFINE_COORDINATE_NODES, *DEFINE_COORDINATE_SYSTEM or *DEFINE_CO- ORDINATE_VECTOR). Available in R3 version of 971 and later. YTFLAG Flag to allow beam to yield in tension: EQ.0.0: beam does not yield in tension, EQ.1.0: beam can yield in tension. ASOFT M1, M2, …, M8 LC1, LC2, …, LC8 LPS1 SFS1 LPS2 SFS2 YMS1 Axial elastic softening factor applied once hinge has formed. When a hinge has formed the stiffness is reduced by this factor. If zero, this factor is ignored. Applied end moment for force versus (strain/change in length) curve. At least one must be defined. A maximum of 8 moments can be defined. The values should be in ascending order. Load curve ID defining axial force versus strain/change in length for the corresponding applied end moment. Define the same number as end moments. Each curve must contain the same number of points. Load curve ID for plastic moment versus rotation about s-axis at node 1. If zero, this load curve is ignored. Scale factor for plastic moment versus rotation curve about s-axis at node 1. Default = 1.0. Load curve ID for plastic moment versus rotation about s-axis at node 2. Default: is same as at node 1. Scale factor for plastic moment versus rotation curve about s-axis at node 2. Default: is same as at node 1. Yield moment about s-axis at node 1 for interaction calculations (default set to 1.0E+20 to prevent interaction). VARIABLE DESCRIPTION YMS2 LPT1 SFT1 LPT2 SFT2 YMT1 YMT2 LPR SFR YMR LYS1 SYS1 LYS2 SYS2 LYT1 Yield moment about s-axis at node 2 for interaction calculations (default set to YMS1). Load curve ID for plastic moment versus rotation about t-axis at node 1. If zero, this load curve is ignored. Scale factor for plastic moment versus rotation curve about t-axis at node 1. Default = 1.0. Load curve ID for plastic moment versus rotation about t-axis at node 2. Default: is the same as at node 1. Scale factor for plastic moment versus rotation curve about t-axis at node 2. Default: is the same as at node 1. Yield moment about t-axis at node 1 for interaction calculations (default set to 1.0E+20 to prevent interactions) Yield moment about t-axis at node 2 for interaction calculations (default set to YMT1) Load curve ID for plastic torsional moment versus rotation. If zero, this load curve is ignored. Scale factor for plastic torsional moment versus rotation (default = 1.0). Torsional yield moment for interaction calculations (default set to 1.0E+20 to prevent interaction) ID of curve defining yield moment as a function of axial force for the s-axis at node 1. Scale factor applied to load curve LYS1. ID of curve defining yield moment as a function of axial force for the s-axis at node 2. Scale factor applied to load curve LYS2. ID of curve defining yield moment as a function of axial force for the t-axis at node 1. SYT1 Scale factor applied to load curve LYT1. LYT2 SYT2 LYR *MAT_MODIFIED_FORCE_LIMITED DESCRIPTION ID of curve defining yield moment as a function of axial force for the t-axis at node 2. Scale factor applied to load curve LYT2. ID of curve defining yield moment as a function of axial force for the torsional axis. SYR Scale factor applied to load curve LYR. HMS1_n Hinge moment for s-axis at node 1. LPMS1_n ID of curve defining plastic moment as a function of plastic rotation for the s-axis at node 1 for hinge moment HMS1_n HMS2_n Hinge moment for s-axis at node 2. LPMS2_n ID of curve defining plastic moment as a function of plastic rotation for the s-axis at node 2 for hinge moment HMS2_n HMT1_n Hinge moment for t-axis at node 1. LPMT1_n ID of curve defining plastic moment as a function of plastic rotation for the t-axis at node 1 for hinge moment HMT1_n HMT2_n Hinge moment for t-axis at node 2. LPMT2_n ID of curve defining plastic moment as a function of plastic rotation for the t-axis at node 2 for hinge moment HMT2_n HMR_n Hinge moment for the torsional axis. LPMR_n ID of curve defining plastic moment as a function of plastic rotation for the torsional axis for hinge moment HMR_n Remarks: This material model is available for the Belytschko resultant beam element only. Plastic hinges form at the ends of the beam when the moment reaches the plastic moment. The plastic moment versus rotation relationship is specified by the user in the form of a load curve and scale factor. The points of the load curve are (plastic rotation in radians, plastic moment). Both quantities should be positive for all points, with the first point being (zero, initial plastic moment). Within this constraint any form of characteristic may be used, including flat or falling curves. Different load curves and scale factors may be specified at each node and about each of the local s and t axes. Axial collapse occurs when the compressive axial load reaches the collapse load. Collapse load versus collapse deflection is specified in the form of a load curve. The points of the load curve are either (true strain, collapse force) or (change in length, collapse force). Both quantities should be entered as positive for all points, and will be interpreted as compressive. The first point should be (zero, initial collapse load). The collapse load may vary with end moment as well as with deflections. In this case several load-deflection curves are defined, each corresponding to a different end moment. Each load curve should have the same number of points and the same deflection values. The end moment is defined as the average of the absolute moments at each end of the beam and is always positive. Stiffness-proportional damping may be added using the damping factor λ. This is defined as follows: 𝜆 = 2 × 𝜉 where ξ is the damping factor at the reference frequency ω (in radians per second). For example if 1% damping at 2Hz is required 𝜆 = 2 × 0.01 2𝜋 × 2 = 0.001592 If damping is used, a small time step may be required. LS-DYNA does not check this so to avoid instability it may be necessary to control the time step via a load curve. As a guide, the time step required for any given element is multiplied by 0.3L⁄cλ when damping is present (L = element length, c = sound speed). Moment Interaction: Plastic hinges can form due to the combined action of moments about the three axes. This facility is activated only when yield moments are defined in the material input. A hinge forms when the following condition is first satisfied. where, ⎜⎛ 𝑀𝑟 ⎟⎞ 𝑀𝑟yield⎠ ⎝ + ⎜⎛ 𝑀𝑠 ⎟⎞ 𝑀𝑠yield⎠ ⎝ + ⎜⎛ 𝑀𝑡 ⎟⎞ 𝑀𝑡yield⎠ ⎝ ≥ 1 𝑀𝑟, 𝑀𝑠, 𝑀𝑡, = current moment 𝑀𝑟yield, 𝑀𝑠yield, 𝑀𝑡yield = yield moment Note that scale factors for hinge behavior defined in the input will also be applied to the yield moments: for example, Msyield in the above formula is given by the input yield moment about the local axis times the input scale factor for the local s axis. For strain- softening characteristics, the yield moment should generally be set equal to the initial peak of the moment-rotation load curve. On forming a hinge, upper limit moments are set. These are given by ⎜⎛𝑀𝑟, ⎝ and similar conditions hold for 𝑀𝑠𝑢𝑝𝑝𝑒𝑟and 𝑀𝑡𝑢𝑝𝑝𝑒𝑟. Thereafter the plastic moments will be given by 𝑀𝑟upper = max ⎟⎞ 2 ⎠ 𝑀𝑟yield 𝑀𝑟𝑝 = min(𝑀𝑟upper, 𝑀𝑟curve) where, 𝑀𝑟p = current plastic moment 𝑀𝑟curve = moment from load curve at the current rotation scaled by the scale factor. 𝑀𝑠𝑝and 𝑀𝑡𝑝 satisfy similar conditions. The effect of this is to provide an upper limit to the moment that can be generated; it represents the softening effect of local buckling at a hinge site. Thus if a member is bent about is local s-axis it will then be weaker in torsion and about its local t-axis. For moments-softening curves, the effect is to trim off the initial peak (although if the curves subsequently harden, the final hardening will also be trimmed off). It is not possible to make the plastic moment vary with the current axial load, but it is possible to make hinge formation a function of axial load and subsequent plastic moment a function of the moment at the time the hinge formed. This is discussed in the next section. Independent plastic hinge formation: In addition to the moment interaction equation, Cards 7 through 18 allow plastic hinges to form independently for the s-axis and t-axis at each end of the beam and also for the torsional axis. A plastic hinge is assumed to form if any component of the current moment exceeds the yield moment as defined by the yield moment vs. axial force curves input on cards 7 and 8. If any of the 5 curves is omitted, a hinge will not form for that component. The curves can be defined for both compressive and tensile axial forces. If the axial force falls outside the range of the curve, the first or last point in the curve will be used. A hinge forming for one component of moment does not effect the other components. Upon forming a hinge, the magnitude of that component of moment will not be permitted to exceed the current plastic moment.. The current plastic moment is obtained by interpolating between the plastic moment vs. plastic rotation curves input on cards 10, 12, 14, 16, or 18. Curves may be input for up to 8 hinge moments, where the hinge moment is defined as the yield moment at the time that the hinge formed. Curves must be input in order of increasing hinge moment and each curve should have the same plastic rotation values. The first or last curve will be used if the hinge moment falls outside the range of the curves. If no curves are defined, the plastic moment is obtain from the curves on cards 4 through 6. The plastic moment is scaled by the scale factors on lines 4 to 6. A hinge will form if either the independent yield moment is exceeded or if the moment interaction equation is satisfied. If both are true, the plastic moment will be set to the minimum of the interpolated value and Mrp. M8 M7 M6 M5 M4 M3 M2 M1M1 Strain (or change in length, see AOPT) Figure M139-1. The force magnitude is limited by the applied end moment. For an intermediate value of the end moment LS-DYNA interpolates between the curves to determine the allowable force value. *MAT_VACUUM This is Material Type 140. This model is a dummy material representing a vacuum in a multi-material Euler/ALE model. Instead of using ELFORM = 12 (under *SECTION_- SOLID), it is better to use ELFORM = 11 with the void material defined as vacuum material instead. Card 1 1 2 3 4 5 6 7 8 Variable MID RHO Type A8 F VARIABLE MID DESCRIPTION Material identification. A unique number or label not exceeding 8 characters must be specified. RHO Estimated material density. This is used only as stability check. Remarks: 1. The vacuum density is estimated. It should be small relative to air in the model (possibly at least 103 to 106 lighter than air). *MAT_RATE_SENSITIVE_POLYMER This is Material Type 141. This model, called the modified Ramaswamy-Stouffer model, is for the simulation of an isotropic ductile polymer with strain rate effects. See references; Stouffer and Dame [1996] and Goldberg and Stouffer [1999]. Uniaxial test data is used to fit the material parameters. Card 1 1 Variable MID Type A8 Card 2 1 Variable Omega Type F VARIABLE MID RO E PR Do N Zo q 2 RO F 2 3 E F 3 4 PR F 4 5 Do F 5 6 N F 6 7 Zo F 7 8 q F 8 DESCRIPTION Material identification. A unique number or label not exceeding 8 characters must be specified. Mass density Elastic modulus. Poisson's ratio Reference strain rate (= 1000 × max strain rate used in the test). Exponent Initial hardness of material . Omega Maximum internal stress. The inelastic strain rate is defined as: *MAT_RATE_SENSITIVE_POLYMER 𝐼 = 𝐷𝑜 exp 𝜀̇𝑖𝑗 ⎡−0.5 ( ⎢ ⎣ 𝑍𝑜 3𝐾2 ) 𝑆𝑖𝑗 − Ω𝑖𝑗 ⎟⎞ √𝐾2 ⎠ ⎤ ⎥ ⎦ ⎜⎛ ⎝ where the 𝐾2 term is given as: 𝐾2 = 0.5(𝑆𝑖𝑗 − Ω𝑖𝑗)(𝑆𝑖𝑗 − Ω𝑖𝑗) and represents the second invariant of the overstress tensor. The elastic components of the strain are added to the inelastic strain to obtain the total strain. The following relationship defines the back stress variable rate: Ω𝑖𝑗 = 𝑞Ω𝑚𝜀̇𝑖𝑗 𝐼 − 𝑞Ω𝑖𝑗𝜀̇𝑒 𝐼 where 𝑞 is a material constant, Ω𝑚 is a material constant that represents the maximum value of the internal stress, and 𝜀̇𝑒 𝐼 is the effective inelastic strain rate. *MAT_TRANSVERSELY_ISOTROPIC_CRUSHABLE_FOAM This is Material Type 142. This model is for an extruded foam material that is transversely isotropic, crushable, and of low density with no significant Poisson effect. This material is used in energy-absorbing structures to enhance automotive safety in low velocity (bumper impact) and medium high velocity (interior head impact and pedestrian safety) applications. The formulation of this foam is due to Hirth, Du Bois, and Weimar and is documented by Du Bois [2001]. Card 1 1 Variable MID Type A8 Card 2 1 2 RO F 2 3 4 5 6 E11 E22 E12 E23 F 3 F 4 F 5 F 6 7 G F 7 8 K F 8 Variable I11 I22 I12 I23 IAA NSYM ANG MU Type I Card 3 1 I 2 I 3 Variable AOPT ISCL MACF Type F I I Card 4 Variable 1 XP Type F 2 YP F 3 ZP F I 4 4 A1 F I 5 5 A2 F I 6 6 A3 F F 7 F 8 7 Variable 1 D1 Type F VARIABLE MID *MAT_TRANSVERSELY_ISOTROPIC_CRUSHABLE_FOAM 2 D2 F 3 D3 F 4 V1 F 5 V2 F 6 V3 F 7 8 DESCRIPTION Material identification. A unique number or label not exceeding 8 characters must be specified. RO E11 E22 E12 E23 G K I11 I22 I12 I23 Mass density Elastic modulus in axial direction. Elastic modulus in transverse direction (E22 = E33). Elastic shear modulus (E12 = E31). Elastic shear modulus in transverse plane. Shear modulus. Bulk modulus for contact stiffness. Load curve for nominal axial stress versus volumetric strain. Load curve ID for nominal transverse stresses versus volumetric strain (I22 = I33). Load curve ID for shear stress component 12 and 31 versus volumetric strain (I12 = I31). Load curve ID for shear stress component 23 versus volumetric strain. IAA NSYM Load curve ID (optional) for nominal stress versus volumetric strain for load at angle, ANG, relative to the material 𝑎-axis. Set to unity for a symmetric yield surface in volumetric compression and tension direction. ANG Angle corresponding to load curve ID, IAA. VARIABLE MU DESCRIPTION Damping coefficient for tensor viscosity which acts in both tension and compression. Recommended values vary between 0.05 to 0.10. If zero, tensor viscosity is not used, but bulk viscosity is used instead. Bulk viscosity creates a pressure as the element compresses that is added to the normal stresses, which can have the effect of creating transverse deformations when none are expected. AOPT Material axes option : EQ.0.0: locally orthotropic with material axes determined by element nodes as shown in Figure M2-1. Nodes 1, 2, and 4 of an element are identical to the nodes used for the definition of a coordinate system as by *DEFINE_- COORDINATE_NODES. EQ.1.0: locally orthotropic with material axes determined by a point in space and the global location of the element center; this is the a-direction. This option is for solid elements only. EQ.2.0: globally orthotropic with material axes determined by vectors defined below, as with *DEFINE_COORDI- NATE_VECTOR. EQ.3.0: locally orthotropic material axes determined by rotating the material axes about the element normal by an angle, BETA, from a line in the plane of the element defined by the cross product of the vector v with the element normal. The plane of a solid element is the midsurface between the inner surface and outer sur- face defined by the first four nodes and the last four nodes of the connectivity of the element, respectively. EQ.4.0: locally orthotropic in cylindrical coordinate system with the material axes determined by a vector v, and an originating point, P, which define the centerline ax- is. This option is for solid elements only. LT.0.0: the absolute value of AOPT is a coordinate system ID number (CID on *DEFINE_COORDINATE_NODES, *DEFINE_COORDINATE_SYSTEM or *DEFINE_CO- ORDINATE_VECTOR). Available in R3 version of 971 and later. ISCL *MAT_TRANSVERSELY_ISOTROPIC_CRUSHABLE_FOAM DESCRIPTION Load curve ID for the strain rate scale factor versus the volumetric strain rate. The yield stress is scaled by the value specified by the load curve. MACF Material axes change flag: EQ.1: No change, default, EQ.2: switch material axes 𝐚 and 𝐛, EQ.3: switch material axes 𝐚 and 𝐜, EQ.4: switch material axes 𝐛 and 𝐜. XP YP ZP Coordinates of point 𝐩 for AOPT = 1 and 4. A1 A2 A3 Components of vector 𝐚 for AOPT = 2. D1 D2 D3 Components of vector 𝐝 for AOPT = 2. V1 V2 V3 Define components of vector v for AOPT = 3 and 4. Remarks: This model behaves in a more physical way for off axis loading the material than, for example, *MAT_HONEYCOMB which can exhibit nonphysical stiffening for loading conditions that are off axis. The curves given for I11, I22, I12 and I23 are used to define a yield surface of Tsai-Wu-type that bounds the deviatoric stress tensor. Hence the elastic parameters E11, E12, E22 and E23 as well as G and K have to be defined in a consistent way. The link ed image cannot be display ed. The file may hav e been mov ed, renamed, or deleted. Verify that the link points to the correct file and location. Figure M142-1. Differences between options NSYM = 1 and NSYM = 0. For the curve definitions volumetric strain 𝜀𝑣 = 1 − 𝑉/𝑉0 is used as the abscissa parameter. If the symmetric option (NSYM = 1) is used, a curve for the first quadrant has to be given only. If NSYM = 0 is chosen, the curve definitions for I11, I22, I12 and I23 (and IAA) have to be in the first and second quadrant as shown in Figure M142-1. Tensor viscosity, which is activated by a nonzero value for MU, is generally more stable than bulk viscosity. A damping coefficient less than 0.01 has little effect, and a value greater than 0.10 may cause numerical instabilities. *MAT_WOOD This is Material Type 143. This is a transversely isotropic material and is available for solid elements. The user has the option of inputting his or her own material properties (<BLANK>), or requesting default material properties for Southern yellow pine (PINE) or Douglas fir (FIR). This model was developed by Murray [2002] under a contract from the FHWA. Available options include: <BLANK> PINE FIR Card 1 1 2 3 4 5 6 7 8 Variable MID RO NPLOT ITERS IRATE GHARD IFAIL IVOL Type A8 F I I I F I I Card 2 for PINE and FIR keyword options. Card 2 1 2 3 4 5 6 7 8 Variable MOIS TEMP QUAL_T QUAL_C UNITS IQUAL Type F F F F I I The following cards 2 through 6 are for option left blank. Card 2 Variable 1 EL Type F 2 ET F 3 4 GLT GTR F F 5 PR F 6 7 Variable 1 XT Type F Card 4 1 2 XC F 2 3 YT F 3 4 YC F 4 *MAT_143 5 6 7 8 SXY SYZ F 5 F 6 7 8 Variable GF1|| GF2|| BFIT DMAX|| GF1┴ GF2┴ DFIT DMAX┴ Type F Card 5 1 F 2 F 3 F 4 F 5 F 6 F 7 F 8 Variable FLPAR FLPARC POWPAR FLPER FLPERC POWPER Type F Card 6 1 F 2 F 3 F 4 F 5 F 6 7 8 Variable NPAR CPAR NPER CPER Type F F F F The remaining cards all keyword options. Card 7 1 2 3 4 5 6 7 8 Variable AOPT MACF BETA Type F I Variable 1 XP Type F Card 9 Variable 1 D1 Type F VARIABLE MID *MAT_WOOD 7 8 7 8 2 YP F 2 D2 F 3 ZP F 3 D3 F 4 A1 F 4 V1 F 5 A2 F 5 V2 F 6 A3 F 6 V3 F DESCRIPTION Material identification. A unique number or label not exceeding 8 characters must be specified. RO Mass density NPLOT Controls what is written as component 7 to the d3plot database. LS-PrePost always blindly labels this component as effective plastic strain.: EQ.1: Parallel damage (default). EQ.2: Perpendicular damage. ITERS Number of plasticity algorithm iterations. The default is one iteration. IRATE Rate effects option: EQ.0: Rate effects model turned off (default). EQ.1: Rate effects model turned on. GHARD Perfect plasticity override. Values greater than or equal to zero are allowed. Positive values model late time hardening in compression (an increase in strength with increasing strain). A zero value models perfect plasticity (no increase in strength with increasing strain). The default is zero. IFAIL Erosion perpendicular to the grain. EQ.0: No (default). EQ.1: Yes (not recommended except for debugging). IVOL Flag to invoke erosion based on negative volume or strain increments greater than 0.01. EQ.0: No, do not apply erosion criteria. EQ.1: Yes, apply erosion criteria. MOIS TEMP QUAL_T Percent moisture content. If left blank, moisture content defaults to saturated at 30%. Temperature in ˚C. If left blank, temperature defaults to room temperature at 20 ˚C Quality factor options. These quality factors reduce the clear wood tension, shear, and compression strengths as a function of grade. EQ.0: Grade 1, 1D, 2, 2D. Predefined strength reduction factors are: Pine: QUAL_T = 0.47 in tension/shear. QUAL_C = 0.63 in compression. Fir: QUAL_T = 0.40 in tension/shear QUAL_C = 0.73 in compression. EQ.-1: DS-65 or SEl STR (pine and fir). Predefined strength reduction factors are: QUAL_T = 0.80 in tension/shear. QUAL_C = 0.93 in compression. EQ.-2: Clear wood. No strength reduction factors are applied: QUAL_T = 1.0. QUAL_C = 1.0. GT.0: User defined quality factor in tension. Values between 0 and 1 are expected. Values greater than one are al- lowed, but may not be realistic. QUAL_C User defined quality factor in compression. This input value is used if Qual_T > 0. Values between 0 and 1 are expected. Values greater than one are allowed, but may not be realistic. If left blank, a default value of Qual_C = Qual_T is used. UNITS Units options: EQ.0: GPa, mm, msec, Kg/mm3, kN. EQ.1: MPa, mm, msec, g/mm3, Nt. EQ.2: MPa, mm, sec, Mg/mm3, Nt. EQ.3: Psi, inch, sec, lb-s2/inch4, lb IQUAL Apply quality factors perpendicular to the grain: EQ.0: Yes (default). EQ.1: No. Parallel normal modulus Perpendicular normal modulus. Parallel shear modulus (GLT = GLR). Perpendicular shear modulus. Parallel major Poisson's ratio. Parallel tensile strength. Parallel compressive strength. Perpendicular tensile strength. Perpendicular compressive strength. Parallel shear strength. Perpendicular shear strength. EL ET GLT GTR PR XT XC YT YC SXY SYZ GF1|| GF2|| Parallel fracture energy in tension. Parallel fracture energy in shear. BFIT Parallel softening parameter. DMAX|| Parallel maximum damage. Perpendicular fracture energy in tension. Perpendicular fracture energy in shear. GF1┴ GF2┴ DFIT Perpendicular softening parameter. DMAX┴ Perpendicular maximum damage. FLPAR Parallel fluidity parameter for tension and shear. FLPARC Parallel fluidity parameter for compression. POWPAR Parallel power. FLPER Perpendicular fluidity parameter for tension and shear. FLPERC Perpendicular fluidity parameter for compression. POWPER Perpendicular power. NPAR Parallel hardening initiation. CPAR NPER CPER AOPT Parallel hardening rate Perpendicular hardening initiation. Perpendicular hardening rate. Material axes option : EQ.0.0: locally orthotropic with material axes determined by element nodes as shown in Figure M2-1. Nodes 1, 2, and 4 of an element are identical to the nodes used for the definition of a coordinate system as by *DEFINE_- COORDINATE_NODES. EQ.1.0: locally orthotropic with material axes determined by a point in space and the global location of the element center; this is the a-direction. This option is for solid elements only. EQ.2.0: globally orthotropic with material axes determined by vectors defined below, as with *DEFINE_COORDI- NATE_VECTOR. EQ.3.0: locally orthotropic material axes determined by rotating the material axes about the element normal by an angle, BETA, from a line in the plane of the element defined by the cross product of the vector v with the element normal. The plane of a solid element is the midsurface between the inner surface and outer surface defined by the first four nodes and the last four nodes of the connectivity of the element, respectively. EQ.4.0: locally orthotropic in cylindrical coordinate system with the material axes determined by a vector v, and an originating point, P, which define the centerline ax- is. This option is for solid elements only. LT.0.0: the absolute value of AOPT is a coordinate system ID number (CID on *DEFINE_COORDINATE_NODES, *DEFINE_COORDINATE_SYSTEM or *DEFINE_CO- ORDINATE_VECTOR). Available in R3 version of 971 and later. MACF Material axes change flag: EQ.1: No change, default, EQ.2: switch material axes a and b, EQ.3: switch material axes a and c, EQ.4: switch material axes b and c. BETA Material angle in degrees for AOPT = 3, may be overridden on the element card, see *ELEMENT_SOLID_ORTHO. XP YP ZP Coordinates of point p for AOPT = 1 and 4. A1 A2 A3 Components of vector a for AOPT = 2. D1 D2 D3 Components of vector d for AOPT = 2. V1 V2 V3 Define components of vector v for AOPT = 3 and 4. Remarks: Material property data is for clear wood (small samples without defects like knots), whereas real structures are composed of graded wood. Clear wood is stronger than graded wood. Quality factors (strength reduction factors) are applied to the clear wood strengths to account for reductions in strength as a function of grade. One quality factor (QUAL_T) is applied to the tensile and shear strengths. A second quality factor (QUAL_C) is applied to the compressive strengths. As a option, predefined quality factors are provided based on correlations between LS-DYNA calculations and test data for pine and fir posts impacted by bogie vehicles. By default, quality factors are applied to both the parallel and perpendicular to the grain strengths. An option is available (IQUAL) to eliminate application perpendicular to the grain. *MAT_PITZER_CRUSHABLE_FOAM This is Material Type 144. This model is for the simulation of isotropic crushable forms with strain rate effects. Uniaxial and triaxial test data have to be used. For the elastic response, the Poisson ratio is set to zero. Card 1 1 Variable MID Type A8 Card 2 1 2 RO F 2 3 K F 3 Variable LCPY LCUYS LCSR Type I I I 6 TY F 6 7 8 SRTV F 7 8 4 G F 4 VC F 5 PR F 5 DFLG F DESCRIPTION VARIABLE MID RO K G PR TY SRTV LCPY LCUYS LCSR Material identification. A unique number or label not exceeding 8 characters must be specified. Mass density Bulk modulus. Shear modulus Poisson's ratio Tension yield. Young’s modulus (E) Load curve ID giving pressure versus volumetric strain, see Figure M75-1. Load curve ID giving uniaxial stress versus volumetric strain, see Figure M75-1. Load curve ID giving strain rate scale factor versus volumetric strain rate. *MAT_PITZER_CRUSHABLE_FOAM DESCRIPTION VC Viscous damping coefficient (.05 < recommended value < .50). DFLG Density flag: EQ.0.0: use initial density EQ.1.0: use current density (larger step size with less mass scaling). Remarks: The logarithmic volumetric strain is defined in terms of the relative volume, 𝑉, as: 𝛾 = −ln(𝑉) In defining the curves the stress and strain pairs should be positive values starting with a volumetric strain value of zero. *MAT_SCHWER_MURRAY_CAP_MODEL This is Material Type 145. *MAT_145 is a Continuous Surface Cap Model and is a three invariant extension of *MAT_GEOLOGIC_CAP_MODEL (*MAT_025) that includes viscoplasticity for rate effects and damage mechanics to model strain softening. The primary references for the model are Schwer and Murray [1994], Schwer [1994], and Murray and Lewis [1994]. *MAT_145 was developed for geomaterials including soils, concrete, and rocks. It is recommended that an updated version of a Continuous Surface Cap Model, *MAT_CSCM (*MAT_159), be used rather than *MAT_SCHWER_- MURRAY_CAP_MODEL (*MAT_145). Warning: no default input parameter values are assumed, but recommendations for the more obscure parameters are provided in the descriptions that follow. Card 1 1 2 3 4 5 6 7 8 Variable MID RO SHEAR BULK GRUN SHOCK PORE Type A8 Card 2 1 F 2 F 3 F 4 F 5 F 6 F 7 8 Variable ALPHA THETA GAMMA BETA EFIT FFIT ALPHAN CALPHA Type F F Card 3 1 Variable RO Type F Card 4 Variable Type 1 W F 2 XO F 2 D1 F F 3 F 4 F 5 F 6 F 7 IROCK SECP AFIT BFIT RDAMO F 3 D2 F F 4 F 5 F 6 F 7 NPLOT EPSMAX CFIT DFIT TFAIL F F F F F F 8 Card 5 1 2 3 4 5 6 7 8 Variable FAILFL DBETA DDELTA VPTAU Type F Card 6 1 F 2 F 3 F 4 5 6 7 8 Variable ALPHA1 THETA1 GAMMA1 BETA1 ALPHA2 THETA2 GAMMA2 BETA2 Type F F F F F F F F VARIABLE MID DESCRIPTION Material identification. A unique number or label not exceeding 8 characters must be specified. RO Mass density SHEAR Shear modulus, G BULK Bulk modulus, K GRUN Gruneisen ratio (typically = 0), Γ SHOCK Shock velocity parameter (typically 0), Sl PORE Flag for pore collapse EQ.0.0: for Pore collapse EQ.1.0: for Constant bulk modulus (typical) ALPHA Shear failure parameter, 𝛼 THETA Shear failure parameter, 𝜃 GAMMA Shear failure parameter, 𝛾 BETA Shear failure parameter, 𝛽 √𝐽′2 = 𝐹𝑒(𝐽1) = 𝛼 − 𝛾exp(−𝛽𝐽1) + 𝜃𝐽1 EFIT Dilitation damage mechanics parameter (no damage = 1) VARIABLE DESCRIPTION FFIT Dilitation damage mechanics parameter (no damage = 0) ALPHAN Kinematic strain hardening parameter, 𝑁𝛼 CALPHAN Kinematic strain hardening parameter, 𝑐𝛼 R0 X0 Initial cap surface ellipticity, R Initial cap surface 𝐽1 (mean stress) axis intercept, 𝑋(𝜅0) IROCK EQ.0: soils (cap can contract) EQ.1: rock/concrete Shear enhanced compaction Ductile damage mechanics parameter (=1 no damage) Ductile damage mechanics parameter (=0 no damage) SECP AFIT BFIT RDAM0 Ductile damage mechanics parameter W D1 D2 Plastic Volume Strain parameter, W Plastic Volume Strain parameter, D1 Plastic Volume Strain parameter, D2 NPLOT EPSMAX CFIT DFIT 𝑃 = 𝑊{1 − exp{−𝐷1[𝑋(𝜅) − 𝑋(𝜅0)] − 𝐷2[(𝑋(𝜅) − 𝑋(𝜅0)]2}} 𝜀𝑉 History variable post-processed as effective plastic strain Maximum permitted strain increment (default = 0) Δ𝜀max = 0.05(𝛼 − 𝑁𝛼 − 𝛾)min( 1 9𝐾) (calculated default) 𝐺, 𝑅 Brittle damage mechanics parameter (=1 no damage) Brittle damage mechanics parameter (=0 no damage) TFAIL Tensile failure stress FAILFL *MAT_SCHWER_MURRAY_CAP_MODEL DESCRIPTION Flag controlling element deletion and effect of damage on stress : EQ.1: 𝜎𝑖𝑗 reduces with increasing damage; element is deleted when fully damaged (default) EQ.-1: 𝜎𝑖𝑗 reduces with increasing damage; element is not deleted EQ.2: 𝑆𝑖𝑗 reduces with increasing damage; element is deleted when fully damaged EQ.-2: 𝑆𝑖𝑗 reduces with increasing damage; element is not deleted DBETA Rounded vertices parameter, Δ𝛽0 DDELTA Rounded vertices parameter, 𝛿 VPTAU Viscoplasticity relaxation time parameter, 𝜏 ALPHA1 Torsion scaling parameter, 𝛼1 𝛼1 < 0 → |𝛼1| = Friction Angle (degrees) THETA1 Torsion scaling parameter, 𝜃1 GAMMA1 Torsion scaling parameter, 𝛾1 BETA1 Torsion scaling parameter, 𝛽1 𝑄1 = 𝛼1 − 𝛾1exp(−𝛽1𝐽1) + 𝜃1𝐽1𝜃2 ALPHA2 Tri-axial extension scaling parameter, 𝛼2 THETA2 Tri-axial extension scaling parameter,𝜃2 GAMMA2 Tri-axial extension scaling parameter, 𝛾2 BETA2 Tri-axial extension scaling parameter, 𝛽2 𝑄2 = 𝛼2 − 𝛾2exp(−𝛽2𝐽1) + 𝜃2𝐽1 Remarks: 1. FAILFL controls whether the damage accumulation applies to either the total stress tensor𝜎𝑖𝑗or the deviatoric stress tensor𝑆𝑖𝑗. When FAILFL = 2, damage does not diminish the ability of the material to support hydrostatic stress. 2. FAILFL also serves as a flag to control element deletion. Fully damaged elements are deleted only if FAILFL is a positive value. When MAT_145 is used with the ALE or EFG solvers, failed elements should not be eroded and so a negative value of FAILFL should be used. Output History Variables: All the output parameters listed in Table M145-1 is available for post-processing using LS-PrePost and its displayed list of History Variables. The LS-DYNA input parameter NEIPH should be set to 26; see for example the keyword input for *DATABASE_EX- TENT_BINARY. PLOT 1 2 3 4 5 6 7 8 9 10 11 12 13 14 15 16 17 18 19 20 21 22 23 24 25 26 Function 𝑋(𝜅) 𝐿(𝜅) 𝑅 𝑅̃ 𝑝 𝜀𝜈 𝐺𝛼 𝛼 𝐽2 𝛽 d Description 𝐽1 intercept of cap surface 𝐽1value at cap-shear surface intercept Cap surface ellipticity Rubin function Plastic volume strain Yield Flag ( = 0 elastic) Number of strain sub-increments Kinematic hardening parameter Kinematic hardening back stress Effective strain rate Ductile damage Ductile damage threshold Strain energy Brittle damage Brittle damage threshold Brittle energy norm 𝐽1 (w/o visco-damage/plastic) 𝐽′2 (w/o visco-damage/plastic) 𝐽′3 (w/o visco-damage/plastic) 𝐽 ̂3(w/o visco-damage/plastic) Lode Angle Maximum damage parameter future variable future variable future variable future variable Table M145-1. Output variables for post-processing using NPLOT parameter. *MAT_SCHWER_MURRAY_CAP_MODEL Gran and Senseny [1996] report the axial stress versus strain response for twelve unconfined compression tests of concrete, used in scale-model reinforced-concrete wall tests. The Schwer & Murray Cap Model parameters provided below were used, see Schwer [2001], to model the unconfined compression test stress-strain response for the nominal 40 MPa strength concrete reported by Gran and Senseny. The basic units for the provided parameters are length in millimeters (mm), time in milliseconds (msec), and mass in grams (g). This base unit set yields units of force in Newtons (N) and pressure in Mega-Pascals (MPa). Example MAT_SCHWER_MURRAY_CAP_MODEL deck Card 1 1 2 3 4 5 6 7 8 Variable MID RO SHEAR BULK GRUN SHOCK PORE Value A8 2.3E-3 1.048E4 1.168E4 0.0 0.0 1. Card 2 1 2 3 4 5 6 7 8 Variable ALPHA THETA GAMMA BETA EFIT FFIT ALPHAN CALPHA Value 190.0 0.0 184.2 2.5E-3 0.999 0.7 2.5 2.5E3 Card 3 Variable 1 R0 2 X0 3 4 5 6 7 8 IROCK SECP AFIT BFIT RDAM0 Value 5.0 100.0 1.0 0.0 0.999 0.3 0.94 Card 4 Variable 1 W 2 D1 3 D2 4 5 6 7 8 NPLOT EPSMAX CFIT DFIT TFAIL Value 5.0E-2 2.5E-4 3.5E-7 23.0 0.0 1.0 300.0 7.0 Card 5 1 2 3 4 5 6 7 8 Variable FAILFG DBETA DDELTA VPTAU Value 1.0 0.0 0.0 0.0 Card 6 1 2 3 4 5 6 7 8 Variable ALPHA1 THETA1 GAMMA1 BETA1 ALPHA2 THETA2 GAMMA2 BETA2 Value 0.747 3.3E-4 0.17 5.0E-2 0.66 4.0E-4 0.16 5.0E-2 User Input Parameters and System of Units Consider the following basic units: Length: 𝐿 (e.g. millimeters - mm ) Mass: M (e.g. grams - g ) Time: T (e.g. milliseconds - ms ) The following consistent unit systems can then be derived using Newton's Law, i.e. 𝐹 = 𝑀𝑎. Force: 𝐹 = 𝑀𝐿/𝑇2 [ g-mm/ms 2= Kg-m/s 2= Newton - N ] Stress: 𝜎 = 𝐹/L2 [ N/mm 2 = 10 6N/m 2 = 10 6 Pascals = MPa ] Density: ρ = M/L3 [ g/mm 3 = 10 6 Kg/m 3 ] User Inputs and Units Card 1 1 2 3 4 5 6 7 8 Variable MID RO SHEAR BULK GRUN SHOCK PORE Units I Density M/L3 Stress: F/L2 Stress: F/L2 Card 2 1 2 3 4 5 6 7 8 Variable ALPHA THETA GAMMA BETA EFIT FFIT ALPHAN CALPHA Units Stress: F/L2 Stress: F/L2 Stress-1: L2/F Stress-½: L/F½ Stress: F/L2 Stress: F/L2 Card 3 Variable 1 R0 2 X0 3 4 5 6 7 8 IROCK SECP AFIT BFIT RDAM0 Units Stress: F/L2 Stress-½: L/F½ Stress½: F½/L Card 4 Variable 1 W 2 D1 3 D2 4 5 6 7 8 NPLOT MAXEPS CFIT DFIT TFAIL Units Stress-1: L2/F Stress-2: L4/F2 Stress-½: L/F½ Stress: F/L2 Card 5 1 2 3 4 5 6 7 8 Variable FAILFG DBETA DDELTA VPTAU Units Angle degrees Time T Card 6 1 2 3 4 5 6 7 8 Variable ALPHA1 THETA1 GAMMA1 BETA1 ALPHA2 THETA2 GAMMA2 BETA2 Units Stress: F/L2 Stress: F/L2 Stress-1: L2/F Stress: F/L2 Stress: F/L2 Stress-1: L2/F *MAT_1DOF_GENERALIZED_SPRING This is Material Type 146. This is a linear spring or damper that allows different degrees-of-freedom at two nodes to be coupled. 3 K F 3 4 C F 4 5 6 7 8 SCLN1 SCLN2 DOFN1 DOFN2 F 5 F 6 I 7 I 8 Card 1 1 Variable MID Type A8 Card 2 1 2 RO F 2 Variable CID1 CID2 Type I I VARIABLE DESCRIPTION MID RO K C Material identification. A unique number or label not exceeding 8 characters must be specified. Mass density, see also volume in *SECTION_BEAM definition. Spring stiffness. Damping constant. SCLN1 Scale factor on force at node 1. Default = 1.0. SCLN2 Scale factor on force at node 2. Default = 1.0. DOFN1 DOFN2 Active degree-of-freedom at node 1, a number between 1 to 6 where 1 is x-translation and 4 is x-rotation. If this parameter is defined in the SECTION_BEAM definition or on the ELEMENT_- BEAM_SCALAR card, then the value here, if defined, is ignored. Active degree-of-freedom at node 2, a number between 1 to 6. If this parameter is defined in the SECTION_BEAM definition or on the ELEMENT_BEAM_SCALAR card, then the value here, if defined, is ignored. CID1 *MAT_1DOF_GENERALIZED_SPRING DESCRIPTION Local coordinate system at node 1. This coordinate system can be overwritten by a local system specified on the *ELEMENT_- BEAM_SCALAR or *SECTION_BEAM keyword input. If no coordinate system is specified, the global system is used. CID2 Local coordinate system at node 2. If CID2 = 0, CID2 = CID1. *MAT_147 This is Material Type 147. This is an isotropic material with damage and is available for solid elements. The model has a modified Mohr-Coulomb surface to determine the pressure dependent peak shear strength. It was developed for applications involving roadbase soils by Lewis [1999] for the FHWA, who extended the work of Abbo and Sloan [1995] to include excess pore water effects. Card 1 1 2 3 4 5 6 7 8 Variable MID RO NPLOT SPGRAV RHOWAT VN GAMMAR INTRMX Type A8 F Default none none Card 2 Variable Type 1 K F 2 G F I 1 3 F F F F none 1.0 0.0 0.0 4 5 6 7 PHIMAX AHYP COH ECCEN AN I 1 8 ET F F F F Default none none none none none none none none Card 3 1 2 3 4 5 6 7 8 Variable MCONT PWD1 PWKSK PWD2 PHIRES DINT VDFM DAMLEV Type F F F F F F F F Default none none none none 0.0 none none none Card 4 1 2 3 4 5 6 7 8 Variable EPSMAX Type F Default none VARIABLE MID DESCRIPTION Material identification. A unique number or label not exceeding 8 characters must be specified. RO Mass density NPLOT Controls what is written as component 7 to the d3plot database. LS-PrePost always blindly labels this component as effective plastic strain. EQ.1: Effective Strain EQ.2: Damage Criterion Threshold EQ.3: Damage (diso) EQ.4: Current Damage Criterion EQ.5: Pore Water Pressure EQ.6: Current Friction Angle (phi) SPGRAV Specific Gravity of Soil used to get porosity. RHOWATt Density of water in model units - used to determine air void strain (saturation) VN Viscoplasticity parameter (strain-rate enhanced strength) GAMMAr Viscoplasticity parameter (strain-rate enhanced strength) ITERMAXx Maximum number of plasticity iterations (default 1) K G Bulk Modulus (non-zero) Shear modulus (non-zero) PHIMAX Peak Shear Strength Angle (friction angle) (radians) VARIABLE DESCRIPTION AHYP Coefficient A for modified Drucker-Prager Surface COH Cohesion ñ Shear Strength at zero confinement (overburden) ECCEN Eccentricity parameter for third invariant effects AN ET MCONT Strain hardening percent of phi max where non-linear effects start Strain Hardening Amount of non-linear effects Moisture Content of Soil (Determines amount of air voids) (0.0 - 1.00) PWD1 Parameter for pore water effects on bulk modulus PWKSK PWD2 PHIRES Skeleton bulk modulus- Pore water parameter ñ set to zero to eliminate effects Parameter for pore water effects on the effective pressure (confinement) The minimum internal friction angle, radians (residual shear strength) DINT Volumetric Strain at Initial damage threshold, EMBED Equation.3 VDFM Void formation energy (like fracture energy) DAMLEV Level of damage that will cause element deletion (0.0 - 1.00) EPSMAX Maximum principle failure strain *MAT_FHWA_SOIL_NEBRASKA This is an option to use the default properties determined for soils used at the University of Nebraska (Lincoln). The default units used for this material are millimeter, millisecond, and kilograms. If different units are desired, the conversion factors must be input. This is Material Type 147. This is an isotropic material with damage and is available for solid elements. The model has a modified Mohr-Coulomb surface to determine the pressure dependent peak shear strength. It was developed for applications involving road base soils. Card 1 1 2 3 4 5 6 7 8 Variable MID FCTIM FCTMAS FCTLEN Type A8 F Default none none I 1 F F F F none 1.0 0.0 0.0 I 1 VARIABLE MID DESCRIPTION Material identification. A unique number or label not exceeding 8 characters must be specified. FCTIM Factor to multiply milliseconds by to get desired time units FCTMAS Factor to multiply kilograms by to get desired mass units FCTLEN Factor to multiply millimeters by to get desired length units Remarks: 1. As an example, if time units of seconds are desired, then FCTIM = 0.001 *MAT_148 This is Material Type 148. This model is for the simulation of thermally equilibrated ideal gas mixtures. This only works with the multi-material ALE formulation (ELFORM = 11 in *SECTION_SOLID). This keyword needs to be used together with *INITIAL_GAS_MIXTURE for the initialization of gas densities and temperatures. When applied in the context of ALE airbag modeling, the injection of inflator gas is done with a *SECTION_POINT_SOURCE_MIXTURE command which controls the injection process. This material model type also has its name start with *MAT_ALE_. For example, an identical material model to this is *MAT_ALE_GAS_MIXTURE (or also, *MAT_ALE_02). Card 1 1 2 3 4 5 6 7 8 Variable MID IADIAB RUNIV Type A8 Default none Remark I 0 5 F 0.0 1 Card 2 for Per mass Calculation. Method (A) RUNIV = blank or 0.0. Card 2 1 2 3 4 5 6 7 8 Variable CVmass1 CVmass2 CVmass3 CVmass4 CVmass5 CVmass6 CVmass7 CVmass8 Type F F F F F F F F Default none none none none none none none none Card 3 for Per mass Calculation. Method (A) RUNIV = blank or 0.0. Card 3 1 2 3 4 5 6 7 8 Variable CPmass1 CPmass 2 CPmass 3 CPmass 4 CPmass 5 CPmass6 CPmass 7 CPmass 8 Type F F F F F F F F Default none none none none none none none none Card 2 for Per Mole Calculation. Method (B) RUNIV is nonzero. Card 2 1 2 3 4 5 6 7 8 Variable MOLWT1 MOLWT2 MOLWT3 MOLWT4 MOLWT5 MOLWT6 MOLWT7 MOLWT8 Type F F F F F F F F Default none none none none none none none none Remark 2 Card 3 for Per Mole Calculation. Method (B) RUNIV is nonzero. Card 3 1 2 3 4 5 6 7 8 Variable CPmole1 CPmole2 CPmole3 CPmole4 CPmole5 CPmole6 CPmole7 CPmole8 Type F F F F F F F F Default none none none none none none none none Remark Card 4 for Per Mole Calculation. Method (B) RUNIV is nonzero. Card 4 Variable 1 B1 Type F 2 B2 F 3 B3 F 4 B4 F 5 B5 F 6 B6 F 7 B7 F 8 B8 F Default none none none none none none none none Remark 2 Card 5 for Per Mole Calculation. Method (B) RUNIV is nonzero. Card 5 Variable 1 C1 Type F 2 C2 F 3 C3 F 4 C4 F 5 C5 F 6 C6 F 7 C7 F 8 C8 F Default none none none none none none none none Remark 2 VARIABLE MID DESCRIPTION Material identification. A unique number or label not exceeding 8 characters must be specified. IADIAB This flag (default = 0) is used to turn ON/OFF adiabatic compression logics for an ideal gas (remark 5). EQ.0: OFF (default) EQ.1: ON RUNIV Universal gas constant in per-mole unit (8.31447 J/(mole*K)). CVmass1 - CVmass8 If RUNIV is BLANK or zero (method A): Heat capacity at constant volume for up to eight different gases in per-mass unit. 𝐶𝑝(𝑇) CPmole kg K mole K mole K2 𝐶 mole K3 Figure M148-1. Standard SI units. VARIABLE DESCRIPTION If RUNIV is BLANK or zero (method A): Heat capacity at constant pressure for up to eight different gases in per-mass unit. If RUNIV is nonzero (method B): Molecular weight of each ideal gas in the mixture (mass-unit/mole). If RUNIV is nonzero (method B): Heat capacity at constant pressure for up to eight different gases in per-mole unit. These are nominal heat capacity values typically at STP. These are denoted by the variable “A” in the equation in remark 2. If RUNIV is nonzero (method B): First order coefficient for a temperature dependent heat capacity at constant pressure for up to eight different gases. These are denoted by the variable “B” in the equation in remark 2. If RUNIV is nonzero (method B): Second order coefficient for a temperature dependent heat capacity at constant pressure for up to eight different gases. These are denoted by the variable “C” in the equation in remark 2. CPmass1 - CPmass8 MOLWT1 - MOLWT8 CPmole1 - CPmole8 B1 - B8 C1 - C8 Remarks: 1. There are 2 methods of defining the gas properties for the mixture. If RUNIV is BLANK or ZERO → Method (A) is used to define constant heat capacities where per-mass unit values of Cv and Cp are input. Only cards 2 and 3 are required for this method. Method (B) is used to define constant or temperature dependent heat capacities where per-mole unit values of Cp are input. Cards 2 - 5 are required for this method. 2. The per-mass-unit, temperature-dependent, constant-pressure heat capacity is 𝐶𝑝(𝑇) = [CPmole + 𝐵 × 𝑇 + 𝐶 × 𝑇2] MOLWT See table M148-1. 3. The initial temperature and the density of the gas species present in a mesh or part at time zero is specified by the keyword *INITIAL_GAS_MIXTURE. 4. The ideal gas mixture is assumed to be thermal equilibrium, that is, all species are at the same temperature (T). The gases in the mixture are also assumed to follow Dalton’s Partial Pressure Law, 𝑃 = ∑ 𝑃𝑖 . The partial pressure of each 𝑅univ 𝑀𝑊 . The individual gas species temper- gas is then 𝑃𝑖 = 𝜌𝑖𝑅gas𝑖 ature equals the mixture temperature. The temperature is computed from the internal energy where the mixture internal energy per unit volume is used, 𝑇 where 𝑅gas𝑖 ngas = ngas 𝑒𝑉 = ∑ 𝜌𝑖𝐶𝑉𝑖 ngas 𝑇𝑖 = ∑ 𝜌𝑖𝐶𝑉𝑖 𝑇 𝑇 = 𝑇𝑖 = 𝑒𝑉 ngas ∑ 𝜌𝑖𝐶𝑉𝑖 In general, the advection step conserves momentum and internal energy, but not kinetic energy. This can result in energy lost in the system and lead to a pressure drop. In *MAT_GAS_MIXTURE the dissipated kinetic energy is au- tomatically converted into heat (internal energy). Thus in effect the total energy is conserved instead of conserving just the internal energy. This numerical scheme has been shown to improve accuracy in some cases. However, the user should always be vigilant and check the physics of the problem closely. 5. As an example consider an airbag surrounded by ambient air. As the inflator gas flows into the bag, the ALE elements cut by the airbag fabric shell elements will contain some inflator gas inside and some ambient air outside. The multi- material element treatment is not perfect. Consequently the temperature of the outside air may be made artificially high after the multi-material element treatment. To prevent the outside ambient air from getting artificially high T, set IDIAB = 1 for the ambient air outside. Simple adiabatic compression equa- tion is then assumed for the outside air. The use of this flag may be needed, but only when that air is modeled by the *MAT_GAS_MIXTURE card. Example: Consider a tank test model where the Lagrangian tank (Part S1) is surrounded by an ALE air mesh (Part H4 = AMMGID 1). There are 2 ALE parts which are defined but initially have no corresponding mesh: part 5 (H5 = AMMGID 2) is the resident gas inside the tank at t = 0, and part 6 (H6 = AMMGID 2) is the inflator gas(es) which is injected into the tank when t > 0. AMMGID stands for ALE Multi-Material Group ID. Please see figure and input below. The *MAT_GAS_MIXTURE (MGM) card defines the gas properties of ALE parts H5 & H6. The MGM card input for both method (A) and (B) are shown. The *INITIAL_GAS_MIXTURE card is also shown. It basically specifies that “AM- MGID 2 may be present in part or mesh H4 at t = 0, and the initial density of this gas is defined in the rho1 position which corresponds to the 1st material in the mixture (or H5, the resident gas).” Example configuration: Cut-off view S1 = tank H4 = AMMG1 = background outside air (initially defined ALE mesh) H5 = AMMG2 = initial gas inside the tank (this has no initial mesh) H6 = AMMG2 = inflator gas(es) injected in (this has no initial mesh) Sample input: $------------------------------------------------------------------------------- *PART H5 = initial gas inside the tank $ PID SECID MID EOSID HGID GRAV ADPOPT TMID 5 5 5 0 5 0 0 *SECTION_SOLID 5 11 0 $------------------------------------------------------------------------------- $ Example 1: Constant heat capacities using per-mass unit. $*MAT_GAS_MIXTURE $ MID IADIAB R_univ $ 5 0 0 $ Cv1_mas Cv2_mas Cv3_mas Cv4_mas Cv5_mas Cv6_mas Cv7_mas Cv8_mas $718.7828911237.56228 $ Cp1_mas Cp2_mas Cp3_mas Cp4_mas Cp5_mas Cp6_mas Cp7_mas Cp8_mas $1007.00058 1606.1117 $------------------------------------------------------------------------------- $ Example 2: Variable heat capacities using per-mole unit. *MAT_GAS_MIXTURE $ MID IADIAB R_univ 5 0 8.314470 $ MW1 MW2 MW3 MW4 MW5 MW6 MW7 MW8 0.0288479 0.02256 $ Cp1_mol Cp2_mol Cp3_mol Cp4_mol Cp5_mol Cp6_mol Cp7_mol Cp8_mol 29.049852 36.23388 $ B1 B2 B3 B4 B5 B6 B7 B8 7.056E-3 0.132E-1 $ C1 C2 C3 C4 C5 C6 C7 C8 -1.225E-6 -0.190E-5 $------------------------------------------------------------------------------- $ One card is defined for each AMMG that will occupy some elements of a mesh set *INITIAL_GAS_MIXTURE $ SID STYPE MMGID T0 4 1 1 298.15 $ RHO1 RHO2 RHO3 RHO4 RHO5 RHO6 RHO7 RHO8 1.17913E-9 *INITIAL_GAS_MIXTURE $ SID STYPE MMGID T0 4 1 2 298.15 $ RHO1 RHO2 RHO3 RHO4 RHO5 RHO6 RHO7 RHO8 1.17913E-9 $------------------------------------------------------------------------------- *MAT_EMMI This is Material Type 151. The Evolving Microstructural Model of Inelasticity (EMMI) is a temperature and rate-dependent state variable model developed to represent the large deformation of metals under diverse loading conditions [Marin 2005]. This model is available for 3D solid elements, 2D solid elements and thick shell forms 3 and 5 . Card 1 1 2 Variable MID RHO Type A8 Card 2 1 F 2 Variable RGAS BVECT Type F Card 3 1 F 2 3 E F 3 D0 F 3 4 PR F 4 QD F 4 5 6 7 8 5 CV F 5 6 7 8 ADRAG BDRAG DMTHTA F 6 F 7 F 8 Variable DMPHI DNTHTA DNPHI THETA0 THETAM BETA0 BTHETA DMR Type F Card 4 1 F 2 F 3 F 4 F 5 F 6 F 7 F 8 Variable DNUC1 DNUC2 DNUC3 DNUC4 DM1 DM2 DM3 DM4 Type F Card 5 1 F 2 F 3 F 4 F 5 F 6 F 7 F 8 Variable DM5 Q1ND Q2ND Q3ND Q4ND CALPHA CKAPPA C1 Type F F F F F F F 1 Variable C2ND Type F Card 7 1 Variable C10 Type F Card 8 1 *MAT_151 2 C3 F 2 A1 F 2 3 C4 F 3 A2 F 3 4 C5 F 4 A3 F 4 5 C6 F 5 A4 F 5 6 7 8 C7ND C8ND C9ND F 6 F 7 F 8 A_XX A_YY A_ZZ F 6 F 7 F 8 Variable A_XY A_YZ A_XZ ALPHXX ALPHYY ALPHZZ ALPHXY ALPHYZ Type F Card 9 1 F 2 F 3 F 4 F 5 F 6 F 7 F 8 Variable ALPHXZ DKAPPA PHI0 PHICR DLBDAG FACTOR RSWTCH DMGOPT Type F Card 10 1 F 2 F 3 F 4 F 5 F 6 F 7 F 8 Variable DELASO DIMPLO ATOL RTOL DINTER Type F F F F *MAT_EMMI Card 11 1 2 3 4 5 6 7 8 Variable Type VARIABLE MID DESCRIPTION Material identification. A unique number or label not exceeding 8 characters must be specified. RHO Material density. E PR Young’s modulus Poisson’s ratio RGAS universal gas constant. BVECT Burger’s vector D0 QD CV pre-exponential diffusivity coefficient activation energy specific heat at constant volume ADRAG drag intercept BDRAG drag coefficient DMTHTA shear modulus temperature coefficient DMPHI shear modulus damage coefficient DNTHTA bulk modulus temperature coefficient DNPHI bulk modulus damage coefficient THETA0 reference temperature THETAM melt temperature BETA0 coefficient of thermal expansion at reference temperature *MAT_151 DESCRIPTION BTHETA thermal expansion temperature coefficient DMR damage rate sensitivity parameter DNUC1 nucleation coefficient 1 DNUC2 nucleation coefficient 2 DNUC3 nucleation coefficient 3 DNUC4 nucleation coefficient 4 DM1 DM2 DM3 DM4 DM5 Q1ND Q2ND Q3ND Q4ND coefficient of yield temperature dependence coefficient of yield temperature dependence coefficient of yield temperature dependence coefficient of yield temperature dependence coefficient of yield temperature dependence dimensionless activation energy for f dimensionless activation energy for rd dimensionless activation energy for Rd dimensionless activation energy Rs CALPHA coefficient for backstress alpha CKAPPA coefficient for internal stress kappa C1 parameter for flow rule exponent n C2ND parameter for transition rate f C3 C4 C5 C6 parameter for alpha dynamic recovery rd parameter for alpha hardening h parameter for kappa dynamic recovery Rd parameter for kappa hardening H C7ND parameter kappa static recovery Rs C8ND C9ND C10 A1 A2 A3 A4 A_XX A_YY A_ZZ A_XY A_YZ A_XZ *MAT_EMMI DESCRIPTION parameter for yield parameter for temperature dependence of flow rule exponent n parameter for static recovery (set = 1) plastic anisotropy parameter plastic anisotropy parameter plastic anisotropy parameter plastic anisotropy parameter initial structure tensor component initial structure tensor component initial structure tensor component initial structure tensor component initial structure tensor component initial structure tensor component ALPHXX initial backstress component ALPHYY initial backstress component ALPHZZ initial backstress component ALPHXY initial backstress component ALPHYZ initial backstress component ALPHXZ initial backstress component DKAPPA initial isotropic internal stress PHI0 initial isotropic porosity PHICR critical cutoff porosity DLBDAG slip system geometry parameter FACTOR fraction of plastic work converted to heat, adiabatic *MAT_151 DESCRIPTION RSWTCH rate sensitivity switch DMGOPT Damage model option parameter EQ.1.0: pressure independent Cocks/Ashby 1980 EQ.2.0: pressure dependent Cocks/Ashby 1980 EQ.3.0: pressure dependent Cocks 1989 DELASO Temperature option EQ.0.0: driven externally EQ.1.0: adiabatic DIMPLO Implementation option flag EQ.1.0: combined viscous drag and thermally activated dislocation motion EQ.2.0: separate viscous drag and thermally activated dislocation motion ATOL RTOL absolute error tolerance for local Newton iteration relative error tolerance for local Newton iteration DNITER maximum number of iterations for local Newton iteration Remarks: ∇ = ℎ 𝐝𝑝 − 𝑟𝑑 𝜀̅ ̇𝑝𝛼̅ 𝛂 ̇𝑝 − 𝑅𝑠𝜅sinh(𝑄𝑠𝜅) 𝜅̇ = (𝐻 − 𝑅𝑑𝜅)𝜀̅ 𝐝p = √ 𝜀̅ ̇𝑝𝐧, 𝜀̅ ̇𝑝 = 𝑓sinh𝑛 [⟨ 𝜎̅̅̅̅̅ 𝜅 + 𝑌 − 1⟩] ̇𝑝 − equation 𝜀̅ 𝑓 = 𝑐2exp ( 𝑄1 ) 𝑛 = 𝑐9 − 𝑐1 𝑌 = 𝑐8𝑌̂(𝜃) 𝛂 − equation 𝜅 − equation 𝑟𝑑 = 𝑐3exp ( −𝑄2 ) 𝑅𝑑 = 𝑐5exp ( −𝑄3 ) ℎ = 𝑐4𝜇̂(𝜃) 𝐻 = 𝑐6𝜇̂(𝜃) 𝑅𝑠 = 𝑐7exp ( −𝑄4 ) 𝑄𝑠 = 𝑐10exp ( −𝑄5 ) Table M151-1. Plasticity Material Functions of EMMI Model. Void growth: 𝜑̇ = √2 (1 − 𝜑)𝐺̂(𝜎̅̅̅̅̅𝑒𝑞, 𝑝̅, 𝜑)𝜀̅ ̇𝑝 𝐺̂(𝜎̅̅̅̅̅𝑒𝑞, 𝑝̅𝜏, 𝜑) = √3 [ (1 − 𝜑)𝑚 + 1 − 1] sinh [ 2(2𝑚 − 1) 2𝑚 + 1 ⟨𝑝̅⟩ 𝜎̅̅̅̅̅𝑒𝑞 ] *MAT_153 This is Material Type 153. This model has two back stress terms for kinematic hardening combined with isotropic hardening and a damage model for modeling low cycle fatigue and failure. Huang [2006] programmed this model and provided it as a user subroutine with the documentation that follows. It is available for beam, shell and solid elements. Card 1 1 Variable MID Type A8 Card 2 1 2 RO F 2 3 E F 3 4 PR F 4 5 6 7 8 SIGY HARDI BETA LCSS F 5 F 6 F 7 I 8 Variable HARDK1 GAMMA1 HARDK2 GAMMA2 SRC SRP HARDK3 GAMMA3 Type F Card 3 1 F 2 F 3 F 4 Variable IDAM IDS IDEP EPSD Type I I I F F 8 F 5 S F F 6 T F F 7 DC F Optional Card 4 Card 4 1 2 3 4 5 6 7 8 Variable HARDK4 GAMMA4 Type F MID RO E PR *MAT_DAMAGE_3 DESCRIPTION Material identification. A unique number or label not exceeding 8 characters must be specified. Mass density, 𝜌 Young’s modulus, E Poisson’s ratio, 𝑣 SIGY Initial yield stress, 𝜎𝑦0 (ignored if LCSS.GT.0) HARDI Isotropic hardening modulus, H (ignored if LCSS.GT.0) BETA LCSS Isotropic hardening parameter, 𝛽. Set 𝛽 = 0 for linear isotropic hardening. (Ignored if LCSS.GT.0 or if HARDI.EQ.0.) Load curve ID defining effective stress vs. effective plastic strain for isotropic hardening. The first abscissa value must be zero corresponding to the initial yield stress. The first ordinate value is the initial yield stress. HARDK1 Kinematic hardening modulus 𝐶1 GAMMA1 Kinematic hardening parameter 𝛾1. Set 𝛾1 = 0 for linear kinematic hardening. Ignored if (HARDK1.EQ.0) is defined. HARDK2 Kinematic hardening modulus 𝐶2 GAMMA2 SRC SRP Kinematic hardening parameter 𝛾2 kinematic hardening. Ignored if (HARDK2.EQ.0) is defined. Set 𝛾2 = 0 for linear . Strain rate parameter, C, for Cowper Symonds strain rate model, see below. If zero, rate effects are not considered. Strain rate parameter, P, for Cowper Symonds strain rate model, see below. If zero, rate effects are not considered. HARDK3 Kinematic hardening modulus 𝐶3 GAMMA3 Kinematic hardening parameter 𝛾3 kinematic hardening. Ignored if (HARDK3.EQ.0) is defined. Set 𝛾3 = 0 for linear . VARIABLE DESCRIPTION IDAM Isotropic damage flag EQ.0: damage is inactivated. IDS, IDEP, EPSD, S, T, DC are ignored. EQ.1: damage is activated IDS Output stress flag EQ.0: undamaged stress is 𝜎̃ output EQ.1: damaged stress is 𝜎̃ (1 − 𝐷) output IDEP Damaged plastic strain EQ.0: plastic strain is accumulated 𝑟 = ∫ 𝜀̅ ̇𝑝𝑙 EQ.1: damaged plastic strain is accumulated 𝑟 = ∫(1 − 𝐷)𝜀̅ ̇𝑝𝑙 EPSD Damage threshold 𝑟𝑑. Damage accumulation begins when 𝑟 > 𝑟𝑑 S T DC Damage material constant S. Default = 𝜎𝑦0 200 ⁄ Damage material constant t. Default = 1 Critical damage value 𝐷𝑐. When damage value reaches critical, the element is deleted from calculation. Default = 0.5 HARDK4 Kinematic hardening modulus 𝐶4 Kinematic hardening parameter 𝛾4 kinematic hardening. Ignored if (HARDK4.EQ.0) is defined. Set 𝛾4 = 0 for linear . GAMMA4 Remarks: This model is based on the work of Lemaitre [1992], and Dufailly and Lemaitre [1995]. It is a pressure-independent plasticity model with the yield surface defined by the function where 𝜎𝑣 is uniaxial yield stress 𝐹 = 𝜎̅̅̅̅̅ − 𝜎𝑦 = 0 𝜎𝑦 = 𝜎𝑦0 + [1 − exp(−𝛽𝑟)] By setting 𝛽 = 0, a linear isotropic hardening is obtained 𝜎𝑦 = 𝜎𝑦0 + 𝐻𝑟 where 𝜎𝑣0 s the initial yield stress. And 𝜎̅̅̅̅̅ is the equivalent von Mises stress, with respect to the deviatoric effective stress where s is deviatoric stress and α is the back stress, which is decomposed into several components se = 𝑑𝑒𝑣[σ̃] − α = s − α and σ̃ is effective stress (undamaged stress), based on Continuum Damage Mechanics model [Lemaitre 1992] α = ∑ αj σ̃ = 1 − 𝐷 where D is the isotropic damage scalar, which is bounded by 0 and 1 0 ≤ 𝐷 ≤ 1 D = 0 represents a damage-free material RVE (representative volume element), while D = 1 represents a fully broken material RVE in two parts. In fact, fracture occurs when 𝐷 = 𝐷𝑐 < 1, modeled as element removal. The evolution of the isotropic damage value related to ductile damage and fracture (the case where the plastic strain or dissipation is much larger than the elastic one, [Lemaitre 1992]) is defined as 𝐷̇ = ⎧ { ⎨ { ⎩ ) ( ̇pl 𝜀̅ 𝑟 > 𝑟𝑑& 𝜎𝑚 𝜎eq otherwise > − where 𝜎𝑚 𝜎𝑒𝑞 is the stress triaxiality, 𝑟𝑑 is damage threshold, S is a material constant, and Y is strain energy density release rate. 𝑌 = εel: 𝐃el: εel Where 𝐃el represents the fourth-order elasticity tensor, εel is elastic strain. And t is a material constant, introduced by Dufailly and Lemaitre [1995], to provide additional degree of freedom for modeling low-cycle fatigue (𝑡 = 1 in Lemaitre [1992]). Dufailly and Lemaitre [1995] also proposed a simplified method to fit experimental results and get S and t. The equivalent Mises stress is defined as 𝜎̅̅̅̅̅(s𝑒) = √ s𝑒: s𝑒 = √ ∥s𝑒∥ The model assumes associated plastic flow ε̇pl = ∂𝐹 ∂σ 𝑑𝜆 = s𝑒 𝜎̅̅̅̅̅ 𝑑𝜆 Where 𝑑𝜆 is the plastic consistency parameter. The evolution of the kinematic component of the model is defined as [Armstrong and Frederick 1966]: α̇𝑗 = ⎧ {{ ⎨ {{ ⎩ 𝐶𝑗ε̇pl − 𝛾𝑗α𝑗𝜀̅ ̇pl IDEP = 0 α̇𝑗 = (1 − 𝐷) ( 𝐶𝑗ε̇pl − 𝛾𝑗α𝑗𝜀̅ ̇pl) IDEP = 1 The damaged plastic strain is accumulated as ̇pl IDEP = 0 ⎧𝑟 = ∫ 𝜀̅ { {⎨ 𝑟 = ∫(1 − 𝐷)𝜀̅ ⎩ ̇pl IDEP = 1 where 𝜀̅ ̇pl is the equivalent plastic strain rate where ε̇pl represents the rate of plastic flow. ̇pl = √ 𝜀̅ ε̇pl: ε̇pl Strain rate is accounted for using the Cowper and Symonds model which scales the yield stress with the factor where 𝜀̇ is the strain rate. 1 + ( 𝑝⁄ ) 𝜀̇ Table 153.1 shows the difference between MAT 153 and MAT 104/105. MAT 153 is less computationally expensive than MAT 104/105. Kinematic hardening, which already exists in MAT 103, is included in MAT 153, but not in MAT 104/105. MAT 153 MAT 104 MAT 105 Computational cost 1.0 3.0 3.0 Isotropic hardening One component Two components One component Kinematic hardening Four components N/A N/A Output stress Damagedplastic strain Accumulation when Isotropic plasticity Anisotropic plasticity Isotropic damage Anisotropic damage IDS = 0 𝜎̃ IDS = 1 𝜎̃ (1 − 𝐷) IDEP = 0 𝑟 = ∫ 𝜀̅ ̇pl IDEP = 1 𝑟 = ∫(1 − 𝐷)𝜀̅ ̇pl 𝜎𝑚 𝜎𝑒𝑞 > − Yes No Yes No 𝜎̃ (1 − 𝐷) 𝜎̃ (1 − 𝐷) 𝑟 = ∫(1 − 𝐷)𝜀̅ ̇pl 𝑟 = ∫(1 − 𝐷)𝜀̅ ̇pl 𝜎1 > 0 𝜎1 > 0 Yes Yes Yes Yes Yes No Yes No Table M153-1. Differences between MAT 153 and MAT 104/105 *MAT_DESHPANDE_FLECK_FOAM This is material type 154 for solid elements. This material is for modeling aluminum foam used as a filler material in aluminum extrusions to enhance the energy absorbing capability of the extrusion. Such energy absorbers are used in vehicles to dissipate energy during impact. This model was developed by Reyes, Hopperstad, Berstad, and Langseth [2002] and is based on the foam model by Deshpande and Fleck [2000]. Card 1 1 2 Variable MID RHO Type A8 F 3 E F 4 PR F 5 6 7 8 ALPHA GAMMA F F Default none none none none none none Card 2 1 2 3 4 5 6 7 8 Variable EPSD ALPHA2 BETA SIGP DERFI CFAIL PFAIL NUM Type F F F F F F F F Default none none none none none none none none VARIABLE MID DESCRIPTION Material identification. A unique number or label not exceeding 8 characters must be specified. RHO Mass density. E PR Young’s modulus. Poisson’s ratio. ALPHA Controls shape of yield surface. GAMMA See remarks. EPSD Densification strain. *MAT_DESHPANDE_FLECK_FOAM DESCRIPTION ALPHA2 See remarks. BETA SIGP See remarks. See remarks. DERFI Type of derivation used in material subroutine EQ.0: Numerical derivation EQ.1: Analytical derivation Failure volumetric strain. Failure principal stress. Must be sustained NUM (>0) timesteps to fail element. CFAIL PFAIL NUM Number of timesteps at or above PFAIL to trigger element failure. Remarks: The yield stress function Φ is defined by: The equivalent stress 𝜎̂ is given by: Φ = 𝜎̂ − 𝜎𝑦 𝜎̂ 2 = 𝜎𝑉𝑀 2 + 𝛼2𝜎𝑚 1 + (𝛼 ) where, 𝜎𝑉𝑀, is the von Mises effective stress: 𝜎𝑉𝑀 = √ σdev: σdev In this equation 𝜎𝑚 and 𝜎 𝑑𝑒𝑣 are the mean and deviatoric stress: The yield stress 𝜎𝑦 can be expressed as: σdev = σ − 𝜎𝑚I 𝜎𝑦 = 𝜎𝑝 + 𝛾 𝜀̂ 𝜀𝐷 + 𝛼2ln ⎡ ⎢ 1 − ( 𝜀̂ ⎣ 𝜀𝐷 ⎤ ⎥ ⎦ ) Here, 𝜎𝑝, 𝛼2, 𝛾 and 𝛽 are material parameters. The densification strain 𝜀𝐷 is defined as: 𝜀𝐷 = −ln ( 𝜌𝑓 𝜌𝑓0 ) where 𝜌𝑓 is the foam density and 𝜌𝑓0 is the density of the virgin material. *MAT_PLASTICITY_COMPRESSION_TENSION_EOS This is Material Type 155. An isotropic elastic-plastic material where unique yield stress versus plastic strain curves can be defined for compression and tension. Also, failure can occur based on a plastic strain or a minimum time step size. Rate effects on the yield stress are modeled either by using the Cowper-Symonds strain rate model or by using two load curves that scale the yield stress values in compression and tension, respectively. Material rate effects, which are independent of the plasticity model, are based on a 6-term Prony series Maxwell mode that generates an additional stress tensor. The viscous stress tensor is superimposed on the stress tensor generated by the plasticity. Pressure is defined by an equation of state, which is required to utilize this model. This model is applicable to solid elements and SPH. Card 1 1 Variable MID 2 RO Type A8 F 3 E F 4 PR F Default none none none none Card 2 1 2 3 4 5 C F 0 5 6 P F 0 6 7 8 FAIL TDEL F 10.E+20 7 F 0 8 Variable LCIDC LCIDT LCSRC LCSRT SRFLAG Type Default Card 3 Variable Type Default I 0 1 PC F 0 I 0 2 PT F 0 I 0 3 I 0 4 F 0 5 6 7 8 PCUTC PCUTT PCUTF SCALEP SCALEE F 0 F 0 F 0 F 0 F 2 3 4 5 6 7 8 Card 4 Variable Type 1 K F Viscoelastic Constant Cards. Card Format for viscoelastic constants. Up to 6 cards may be input. A keyword card (with a “*” in column 1) terminates this input if less than 6 cards are used. Optional Variable Type 1 GI F VARIABLE MID RO E PR C P 2 3 4 5 6 7 8 BETAI F DESCRIPTION Material identification. A unique number or label not exceeding 8 characters must be specified. Mass density. Young’s modulus. Poisson’s ratio. Strain rate parameter, C, see formula below. Strain rate parameter, P, see formula below. FAIL Failure flag. LT.0.0: User defined failure subroutine, matusr_24 in dyn21.F, is called to determine failure EQ.0.0: Failure is not considered. This option is recommended if failure is not of interest since many calculations will be saved. GT.0.0: Plastic strain to failure. When the plastic strain reaches this value, the element is deleted from the calculation. TDEL Minimum time step size for automatic element deletion. LCIDC LCIDT LCSRC LCSRT *MAT_PLASTICITY_COMPRESSION_TENSION_EOS DESCRIPTION Load curve ID defining yield stress versus effective plastic strain in compression. Load curve ID defining yield stress versus effective plastic strain in tension. Optional load curve ID defining strain rate scaling effect on yield stress when the material is in compression. Optional load curve ID defining strain rate scaling effect on yield stress when the material is in tension. SRFLAG Formulation for rate effects: EQ.0.0: Total strain rate, EQ.1.0: Deviatoric strain rate. PC PT PCUTC PCUTT Compressive mean stress (pressure) at which the yield stress follows load curve ID, LCIDC. If the pressure falls between PC and PT a weighted average of the two load curves is used. Tensile mean stress at which the yield stress follows load curve ID, LCIDT. Pressure cut-off in compression. When the pressure cut-off is reached the deviatoric stress tensor is set to zero. The compressive pressure is not, however, limited to PCUTC. Like the yield stress, PCUTC is scaled to account for rate effects. Pressure cut-off in tension. When the pressure cut-off is reached the deviatoric stress tensor and tensile pressure is set to zero. Like the yield stress, PCUTT is scaled to account for rate effects. PCUTF Pressure cut-off flag. EQ.0.0: Inactive, EQ.1.0: Active. SCALEP Scale factor applied to the yield stress after the pressure cut-off is reached in either compression or tension. If SCALEP = 0 (default), the deviatoric stress is set to zero after the cut-off is reached. VARIABLE SCALEE K GI DESCRIPTION Scale factor applied to the yield stress after the strain exceeds the failure strain set by FAIL. If SCALEE = 0 (default), the deviatoric strain is set to zero if the failure strain is exceeded. IF both SCALEP > 0 and SCALEE > 0 and both failure conditions are met, then the minimum scale factor is used. Optional bulk modulus for the viscoelastic material. If nonzero a Kelvin type behavior will be obtained. Generally, K is set to zero. Optional shear relaxation modulus for the ith term BETAI Optional shear decay constant for the ith term Remarks: The stress strain behavior follows a different curve in compression than it does in tension. Tension is determined by the sign of the mean stress where a positive mean stress (i.e., a negative pressure) is indicative of tension. Two curves must be defined giving the yield stress versus effective plastic strain for both the tension and compression regimes. Mean stress is an invariant which can be expressed as (σx + σy + σz)/3. PC and PT define a range of mean stress values within which interpolation is done between the tensile yield surface and compressive yield surface. PC and PT are not true material properties but are just a numerical convenience so that the transition from one yield surface to the other is not abrupt as the sign of the mean stress changes. Both PC and PT are input as positive values as it is implied that PC is a compressive mean stress value and PT is tensile mean stress value. Strain rate may be accounted for using the Cowper and Symonds model which scales the yield stress with the factor: where 𝜀̇ is the strain rate, 1 + ( 𝑝⁄ ) 𝜀̇ 𝜀̇ = √𝜀̇𝑖𝑗𝜀̇𝑖𝑗. *MAT_PLASTICITY_COMPRESSION_TENSION_EOS History Variable Description 4 5 6 7 Tensile pressure cutoff (set to zero if tensile or compressive failure occurs) The cutoff flag, initially equals 1, set to 0 if tensile or compressive failure occurs The failure mode flag EQ.0: if no failure EQ.1: if compressive failure EQ.2: if tensile failure EQ.3: if failure by plastic strain The current flow stress *MAT_156 This is material type 156 for truss elements. This material is a Hill-type muscle model with activation and a parallel damper. Also, see *MAT_SPRING_MUSCLE where a description of the theory is available. Card 1 1 Variable MID 2 RO 3 4 5 6 7 8 SNO SRM PIS SSM CER DMP Type A8 F F F F F F F Default Card 2 1 2 3 4 5 6 7 8 Variable ALM SFR SVS SVR SSP Type F F F F F Default 0.0 1.0 1.0 1.0 0.0 VARIABLE DESCRIPTION MID RO SNO SRM PIS Material identification. A unique number or label not exceeding 8 characters must be specified. Material density in the initial undeformed configuration. Initial stretch ratio, 𝑙0 𝑙orig , i.e., the length as defined by the nodal points at t = 0 divided by the original initial length. The density for the nodal mass calculation is RO/SNO, or 𝑙orig 𝑙0 𝜌. Maximum strain rate. Peak isometric stress corresponding to the dimensionless value of unity in the dimensionless stress versus strain function, see SSP below. SSM CER DMP ALM *MAT_MUSCLE DESCRIPTION Strain when the dimensionless stress versus strain function, SSP below, reaches its maximum stress value. Constant, governing the exponential rise of SSP. Required if SSP = 0. Damping constant (stress × time units). Activation level vs. time. LT.0: absolute value gives load curve ID GE.0: constant value of ALM is used SFR Scale factor for strain rate maximum vs. activation level, 𝑎(𝑡). LT.0: absolute value gives load curve ID GE.0: constant value of 1.0 is used SVS SVR Active dimensionless tensile stress vs. the stretch ratio, 𝑙orig . LT.0: absolute value gives load curve ID GE.0: constant value of 1.0 is used Active dimensionless tensile stress vs. the normalized strain rate, ̇. 𝜀̅ LT.0: absolute value gives load curve ID GE.0: constant value of 1.0 is used SSP Isometric dimensionless stress vs. the stretch ratio, 𝑙orig for the parallel elastic element. LT.0: absolute value gives load curve ID or table ID EQ.0: exponential function is used GT.0: constant value of 0.0 is used Remarks: The material behavior of the muscle model is adapted from *MAT_S15, the spring muscle model and treated here as a standard material. The initial length of muscle is calculated automatically. The force, relative length and shortening velocity are replaced by stress, strain and strain rate. A new parallel damping element is added. The strain 𝜀 and normalized strain rate 𝜀̅ ̇ are defined respectively as and, 𝜀 = 𝑙orig − 1 = SNO × 𝑙0 − 1 𝜀̅ ̇ = 𝑙orig 𝜀̇ 𝜀̇max = SNO × 𝑙0 × 𝜀̇ SFR × SRM where 𝜀̇ = ∆𝜀/∆𝑡 (current strain increment divided by current time step), l = current muscle length, and 𝑙orig = original muscle length. From the relation above, it is known: 𝑙orig = 𝑙0 1 + 𝜀0 where 𝜀0 = SNO − 1 and 𝑙0 = muscle length at time 0. Stress of Contractile Element is: 𝜎1 = 𝜎max𝑎(𝑡)𝑓 ( 𝑙orig ) 𝑔(𝜀̅ ̇) where 𝜎max = PIS, 𝑎(𝑡) = ALM, 𝑓 (𝑙/𝑙orig) = SVS, and 𝑔(𝜀̅ ̇) = SVR. Stress of Passive Element is: 𝜎2 = ⎧ {{{ ⎨ {{{ ⎩ 𝜎maxℎ ( ̇, 𝜎maxℎ (𝜀̅ ) 𝑙orig 𝑙orig for curve ) for table where ℎ = SSP. For SSP < 0, the absolute value gives a load curve ID or table ID. The load curve defines isometric dimensionless stress ℎ versus stretch ratio 𝑙/𝑙orig. The table ̇ a load curve giving the isometric dimension- defines for each normalized strain rate 𝜀̅ less stress ℎ versus stretch ratio 𝑙/𝑙orig for that rate. *MAT_MUSCLE ⎜⎜⎜⎜⎛ ⎝ ⁄ 𝑙orig = ⎟⎟⎟⎟⎞ ⎠ exp(CER) − 1 ⎧0 { { { { { { ⎨ { { { { { { ⎩ SSM ⁄ < 1 𝑙orig [ exp ( CER SSM 𝜀) − 1] ⁄ ≥ 1 CER ≠ 0 𝑙orig ⁄ ≥ 1 CER = 0 𝑙orig Stress of Damping Element is: Total Stress is: σ3 = DMP × 𝑙orig ε̇ 𝜎 = 𝜎1 + 𝜎2 + 𝜎3 *MAT_ANISOTROPIC_ELASTIC_PLASTIC This is Material Type 157. This material model is a combination of the anisotropic elastic material model (MAT_002) and the anisotropic plastic material model (MAT_- 103_P). Also, brittle orthotropic failure based on a phenomenological Tsai-Wu criterion can be defined. Card 1 1 Variable MID Type A8 Card 2 1 2 RO F 2 3 4 5 6 7 8 SIGY LCSS QR1 CR1 QR2 CR2 F 3 F 4 F 5 F 6 F 7 F 8 Variable C11 C12 C13 C14 C15 C16 C22 C23 Type F Card 3 1 F 2 F 3 F 4 F 5 F 6 F 7 F 8 Variable C24 C25 C26 C33 C34 C35 C36 C44 Type F Card 4 1 F 2 F 3 F 4 F 5 F 6 F 7 F 8 Variable C45 C46 C55 C56 C66 R00 or F R45 or G R90 or H Type F Card 5 1 F 2 F 3 F 4 F 5 Variable S11 or L S22 or M S33 or N S12 AOPT Type F F F F F F 6 VP F F 7 F 8 MACF Variable 1 XP Type F Card 7 Variable 1 V1 Type F *MAT_ANISOTROPIC_ELASTIC_PLASTIC 2 YP F 2 V2 F 3 ZP F 3 V3 F 4 A1 F 4 D1 F 5 A2 F 5 D2 F 6 A3 F 6 D3 F 7 8 EXTRA F 8 7 BETA IHIS F F Two additional cards for EXTRA = 1 or 2. Card 8 Variable 1 XT Type F Card 9 Variable 1 ZT Type F 2 XC F 2 ZC F 3 YT F 3 4 YC F 4 5 6 7 8 SXY FF12 NCFAIL F 5 F 6 7 F 8 SYZ SZX FF23 FF31 F F F F VARIABLE DESCRIPTION MID RO SIGY LCSS Material identification. A unique number or label not exceeding 8 characters must be specified. Mass density. Initial yield stress Load curve ID or Table ID. Load Curve. When LCSS is a Load curve ID, it is taken as defining effective stress versus effective plastic strain. If defined VARIABLE DESCRIPTION QR1, CR1, QR2, and CR2 are ignored. Tabular Data. The table ID defines for each strain rate value a load curve ID giving the stress versus effective plastic strain for that rate, See Figure M24-1. When the strain rate falls below the minimum value, the stress versus effective plastic strain curve for the lowest value of strain rate is used. Likewise, when the strain rate exceeds the maximum value the stress versus effective plastic strain curve for the highest value of strain rate is used. Logarithmically Defined Tables. If the first stress-strain curve in the table corresponds to a negative strain rate, LS-DYNA assumes that the natural logarithm of the strain rate value is used for all stress-strain curves. Since the tables are internally discretized to equally space the points, natural logarithms are necessary, for example, if the curves correspond to rates from 10−4 to 104. Computing natural logarithms can substantially increase the computational time on certain computer architectures. Isotropic hardening parameter Isotropic hardening parameter Isotropic hardening parameter Isotropic hardening parameter The i, j term in the 6 × 6 anisotropic constitutive matrix. Note that 1 corresponds to the a material direction, 2 to the b material direction, and 3 to the c material direction. 𝑅00 for shell (Default = 1.0) 𝑅45 for shell (Default = 1.0) 𝑅90 for shell (Default = 1.0) 𝐹 for brick (Default = 1 2⁄ ) 𝐺 for brick (Default = 1 2⁄ ) 𝐻 for brick (Default = 1 2⁄ ) 𝐿 for brick (Default = 3 2⁄ ) 𝑀 for brick (Default = 3 2⁄ ) QR1 CR1 QR2 CR2 Cij R00 R45 R90 F G H L N S11 S22 S33 S12 *MAT_ANISOTROPIC_ELASTIC_PLASTIC DESCRIPTION 𝑁 for brick (Default = 3 2⁄ ) Yield stress in local-x direction (shells only). This input is ignored when R00, R45, R90 > 0. Yield stress in local-y direction (shells only). This input is ignored when R00, R45, R90 > 0. Yield stress in local-z direction (shells only). This input is ignored when R00, R45, R90 > 0. Yield stress in local-xy direction (shells only). This input is ignored when R00, R45, R90 > 0. AOPT Material axes option . Available in R3 version of 971 and later. VARIABLE DESCRIPTION VP Formulation for rate effects: EQ.0.0: scale yield stress (default), EQ.1.0: viscoplastic formulation. MACF Material axes change flag for brick elements: EQ.1: No change, default, EQ.2: switch material axes 𝑎 and 𝑏, EQ.3: switch material axes 𝑎 and 𝑐, EQ.4: switch material axes 𝑏 and 𝑐. XP, YP, ZP coordinates of point 𝐩 for AOPT = 1 and 4. A1, A2, A3 components of vector 𝐚 for AOPT = 2. D1, D2, D3 components of vector 𝐝 for AOPT = 2. V1, V2, V3 components of vector 𝐯 for AOPT = 3 and 4. BETA Material angle in degrees for AOPT = 0 (shells only) and AOPT = 3. BETA may be overridden on the element card, see *ELEMENT_SHELL_BETA and *ELEMENT_SOLID_ORTHO. IHIS Flag for material properties initialization. EQ.0: material properties defined in Cards 1-5 are used GE.1: Use *INITIAL_STRESS_SOLID/SHELL initialize material properties on an element-by-element basis for solid or shell elements, respectively . to EXTRA Flag to input further data : EQ.1.0: Tsai-Wu failure criterion parameters (cards 8 and 9) EQ.2.0: Tsai-Hill failure criterion parameters (cards 8 and 9) XT Longitudinal tensile strength, a-axis. GT.0.0: constant value LT.0.0: Load curve ID = (-XT) which defines the longitudinal tensile strength vs. strain rate. If the first strain rate value in the curve is negative, it is assumed that all strain rate values are given as natural logarithm of the strain rate. *MAT_ANISOTROPIC_ELASTIC_PLASTIC DESCRIPTION XC Longitudinal compressive strength, a-axis (positive value). GT.0.0: constant value LT.0.0: Load curve ID = (-XC) which defines the longitudinal compressive strength vs. strain rate. If the first strain rate value in the curve is negative, it is assumed that all strain rate values are given as natural logarithm of the strain rate. YT Transverse tensile strength, b-axis. GT.0.0: constant value LT.0.0: Load curve ID = (-YT) which defines the transverse tensile strength vs. strain rate. If the first strain rate value in the curve is negative, it is assumed that all strain rate values are given as natural logarithm of the strain rate. YC Transverse compressive strength, b-axis (positive value). GT.0.0: constant value LT.0.0: Load curve ID = (-YC) which defines the transverse compressive strength vs. strain rate. If the first strain rate value in the curve is negative, it is assumed that all strain rate values are given as natural logarithm of the strain rate. SXY Shear strength, ab-plane. GT.0.0: constant value LT.0.0: Load curve ID = (-SXY) which defines the shear strength vs. strain rate. If the first strain rate value in the curve is negative, it is assumed that all strain rate values are given as natural logarithm of the strain rate. FF12 NCFAIL Scale factor between -1 and +1 for interaction term F12, see Remarks. Number of timesteps to reduce stresses until element deletion. The default is NCFAIL = 10. VARIABLE DESCRIPTION ZT Transverse tensile strength, c-axis (solid elements only). GT.0.0: constant value LT.0.0: Load curve ID = (-ZT) which defines the transverse tensile strength vs. strain rate. If the first strain rate value in the curve is negative, it is assumed that all strain rate values are given as natural logarithm of the strain rate. ZC Transverse compressive strength, c-axis (positive value) (solid elements only). GT.0.0: constant value LT.0.0: Load curve ID = (-ZC) which defines the transverse compressive strength vs. strain rate. If the first strain rate value in the curve is negative, it is assumed that all strain rate values are given as natural logarithm of the strain rate. SYZ Shear strength, bc-plane (solid elements only). GT.0.0: constant value LT.0.0: Load curve ID = (-SYZ) which defines the shear strength vs. strain rate. If the first strain rate value in the curve is negative, it is assumed that all strain rate values are given as natural logarithm of the strain rate. SZX Shear strength, ca-plane (solid elements only). GT.0.0: constant value LT.0.0: Load curve ID = (-SZX) which defines the shear strength vs. strain rate. If the first strain rate value in the curve is negative, it is assumed that all strain rate values are given as natural logarithm of the strain rate. FF23 FF31 Scale factor between -1 and +1 for interaction term F23, see Remarks (solid elements only). Scale factor between -1 and +1 for interaction term F31, see Remarks (solid elements only). Description of IHIS (Solid Elements): Several of this material’s parameters may be overwritten on an element-by-element basis through history variables using the *INITIAL_STRESS_SOLID keyword. Bitwise (binary) expansion of IHIS determines which material properties are to be read: IHIS = 𝑎3 × 8 + 𝑎2 × 4 + 𝑎1 × 2 + 𝑎0, where each 𝑎𝑖 is a binary flag set to either 1 or 0. The 𝑎𝑖 are interpreted according to the following table. Flag Description Variables 𝑎0 Material directions 𝑞11, 𝑞12, 𝑞13, 𝑞31, 𝑞32, 𝑞33 𝑎1 𝑎2 𝑎3 Anisotropic stiffness Cij Anisotropic constants F, G, H, L, M, N Stress-strain Curve LCSS # 6 21 6 1 The NHISV field on *INITIAL_STRESS_SOLID must be set equal to the sum of the number of variables to be read in, which depends on IHIS (and the 𝑎𝑖): NHISV = 6𝑎0 + 21𝑎1 + 6𝑎2 + 𝑎3. Then, in the following order, *INITIAL_STRESS_SOLID processes the history variables, HISVi, as: 1. 2. 3. 4. 6 material direction parameters when 𝑎0 = 1 21 anisotropic stiffness parameters when 𝑎1 = 1 6 anisotropic constants when 𝑎2 = 1 1 parameters when 𝑎3 = 1 The 𝑞𝑖𝑗 terms are the first and third rows of a rotation matrix for the rotation from a co- rotational element’s system and the 𝑎-𝑏-𝑐 material directions. The 𝑐𝑖𝑗 terms are the upper triangular terms of the symmetric stiffness matrix, 𝑐11, 𝑐12, 𝑐13, 𝑐14, 𝑐15, 𝑐16, 𝑐22, 𝑐23, 𝑐24, 𝑐25, 𝑐26, 𝑐33, 𝑐34, 𝑐35, 𝑐36, 𝑐44, 𝑐45, 𝑐46, 𝑐55, 𝑐56, and 𝑐66. Description of IHIS (Shell Elements): Several of this material’s parameters may be overwritten on an element-by-element basis through history variables using the *INITIAL_STRESS_SHELL keyword. Bitwise (binary) expansion of IHIS determines which material properties are to be read: IHIS = 𝑎4 × 16 + 𝑎3 × 8 + 𝑎2 × 4 + 𝑎1 × 2 + 𝑎0, where each 𝑎𝑖 is a binary flag set to either 1 or 0. The 𝑎𝑖 are interpreted according to the following table. Flag Description Variables 𝑎0 Material directions Anisotropic stiffness 𝑞1, 𝑞2 Cij Anisotropic constants 𝑟00, 𝑟45, 𝑟90 Stress-strain Curve LCSS Strength limits XT, XC, YT, YC, SXY 𝑎1 𝑎2 𝑎3 𝑎4 # 2 21 3 1 5 The NHISV field on *INITIAL_STRESS_SHELL must be set equal to the sum of the number of variables to be read in, which depends on IHIS (and the 𝑎𝑖): NHISV = 2𝑎0 + 21𝑎1 + 3𝑎2 + 𝑎3 + 5𝑎4. Then, in the following order, *INITIAL_STRESS_SHELL processes the history variables, HISVi, as: 5. 6. 7. 8. 9. 2 material direction parameters when 𝑎0 = 1 21 anisotropic stiffness parameters when 𝑎1 = 1 3 anisotropic constants when 𝑎2 = 1 1 parameters when 𝑎3 = 1 5 strength parameters when 𝑎4 = 1 The 𝑞𝑖 terms are the material direction cosine and sinus for the rotation from a co- rotational element’s system to the 𝑎-𝑏-𝑐 material directions. The 𝑐𝑖𝑗 terms are the upper triangular terms of the symmetric stiffness matrix, 𝑐11, 𝑐12, 𝑐13, 𝑐14, 𝑐15, 𝑐16, 𝑐22, 𝑐23, 𝑐24, 𝑐25, 𝑐26, 𝑐33, 𝑐34, 𝑐35, 𝑐36, 𝑐44, 𝑐45, 𝑐46, 𝑐55, 𝑐56, and 𝑐66. Tsai-Wu failure criterion (EXTRA = 1): Brittle failure with different strengths in tension and compression in all main material directions can be invoked with EXTRA = 1 and the definition of corresponding parameters on Cards 8 and 9. The model used is the phenomenological Tsai-Wu failure criterion which requires that + XT ⋅ XC ( − − XT YC ) 𝜎𝑎𝑎 + ( XC YT ⋅ YC ZC SYZ2 𝜎𝑏𝑐 +2 ⋅ 𝐹12 ⋅ 𝜎𝑎𝑎𝜎𝑏𝑏 + 2 ⋅ 𝐹23 ⋅ 𝜎𝑏𝑏𝜎𝑐𝑐 + 2 ⋅ 𝐹31 ⋅ 𝜎𝑐𝑐𝜎𝑎𝑎 < 1 YT ZT ⋅ ZC SXY2 𝜎𝑎𝑏 ) 𝜎𝑏𝑏 + ( ZT ) 𝜎𝑐𝑐 2 + 2 + 2 + 2 + 𝜎𝑏𝑏 𝜎𝑐𝑐 − 𝜎𝑎𝑎 2 + 2 SZX2 𝜎𝑐𝑎 for the 3-dimensional case (solid elements) with three planes of symmetry with respect to the material coordinate system. The interaction terms 𝐹12, 𝐹23, and 𝐹31 are given by 𝐹12 = FF12 ⋅ √ ZT⋅ZC⋅XT⋅XC For the 2-dimensional case of plane stress (shell elements) this expression reduces to: XT⋅XC⋅YT⋅YC , 𝐹23 = FF23 ⋅ √ YT⋅YC⋅ZT⋅ZC , 𝐹31 = FF31 ⋅ √ ( XT − XC ) 𝜎𝑎𝑎 + ( YC ) 𝜎𝑏𝑏 + XT ⋅ XC 2 + 𝜎𝑎𝑎 YT ⋅ YC 2 𝜎𝑏𝑏 − YT SXY2 𝜎𝑎𝑏 + 2 + 2 ⋅ 𝐹12 ⋅ 𝜎𝑎𝑎𝜎𝑏𝑏 < 1 If these conditions are violated, then the stress tensor will be reduced to zero over NCFAIL time steps and then the element gets eroded. A small value for NCFAIL (< 50) is recommended to avoid unphysical behavior, the default is 10. The default values for the strengths XT, XC, YT, YC, ZT, ZC, SXY, SYZ, and SZX are 1e20, i.e. basically no limits. The scale factors FF12, FF23, and FF31 for the interaction terms are zero by default. Tsai-Hill failure criterion (EXTRA = 2): Brittle failure with different strengths in tension and compression in all main material directions can be invoked with EXTRA = 2 and the definition of corresponding parameters on Cards 8 and 9 (FF12, FF23 and FF31 are not used in this model). The model based on the HILL criterion which can be written as (G + H)σaa 2 + (F + H)σbb 2 + 2Mσca 2 + (F + G)σcc 2 < 1 2 + 2Lσbc +2Nσab 2 − 2Hσaaσbb − 2F σbbσcc − 2Gσccσaa for the 3-dimensional case. The constants H,F,G,N,L,M can be expressed in terms of the strength limits (which then becomes the TSAI-HILL criterion), where the current stress state defines whether the compressive or the tensile strength limit will enter into the equation: G + H = 2 ; F + H = Xi 2 ; F + G = Yi 2 ; 2𝑁 = Zi 𝑆𝑋𝑌2 ; 2𝐿 = 𝑆𝑌𝑍2 ; 2𝑁 = 𝑆𝑍𝑋2 2 − 1 2 + 1 2) ; G= 0.5 ⋅ ( 1 2 − 1 2 + 1 2) ; F= 0.5 ⋅ ( 1 2 − 1 2 + 1 H= 0.5 ⋅ ( 1 2) 𝑌𝑖 𝑍𝑖 𝑋𝑖 𝑋𝑖 𝑍𝑖 𝑌𝑖 𝑍𝑖 𝑌𝑖 𝑋𝑖 𝑋𝑖 = { 𝑋𝑇 𝑖𝑓 𝜎𝑎𝑎 > 0 𝑋𝐶 𝑖𝑓 𝜎𝑎𝑎 < 0 ; 𝑌𝑖 = { 𝑌𝑇 𝑖𝑓 𝜎𝑏𝑏 > 0 𝑌𝐶 𝑖𝑓 𝜎𝑏𝑏 < 0 ; 𝑍𝑖 = { 𝑍𝑇 𝑖𝑓 𝜎𝑐𝑐 > 0 𝑍𝐶 𝑖𝑓 𝜎𝑐𝑐 < 0 For the 2-dimensional case of plane stress (shell elements) the TSAI-HILL criterion reduces to: (G + H)σaa 2 + (F + H)σbb 2 − 2Hσaaσbb + 2Nσab 2 < 1 with G + H = 2 ; F + H = Xi 2 ; H = 0.5 ⋅ ( Yi 2) ; 2𝑁 = Xi 𝑆𝑋𝑌2 If these conditions are violated, then the stress tensor will be reduced to zero over NCFAIL time steps and then the element gets eroded. A small value for NCFAIL (< 50) is recommended to avoid unphysical behavior, the default is 10. The default values for the strengths XT, XC, YT, YC, ZT, ZC, SXY, SYZ, and SZX are 1e20, i.e. basically no limits. *MAT_RATE_SENSITIVE_COMPOSITE_FABRIC This is Material Type 158. Depending on the type of failure surface, this model may be used to model rate sensitive composite materials with unidirectional layers, complete laminates, and woven fabrics. A viscous stress tensor, based on an isotropic Maxwell model with up to six terms in the Prony series expansion, is superimposed on the rate independent stress tensor of the composite fabric. The viscous stress tensor approach should work reasonably well if the stress increases due to rate affects are up to 15% of the total stress. This model is implemented for both shell and thick shell elements. The viscous stress tensor is effective at eliminating spurious stress oscillations. Card 1 1 Variable MID Type A8 Card 2 1 2 RO F 2 3 EA F 3 4 EB F 4 5 6 7 8 (EC) PRBA TAU1 GAMMA1 F 5 F 6 F 7 F 8 Variable GAB GBC GCA SLIMT1 SLIMC1 SLIMT2 SLIMC2 SLIMS Type F Card 3 1 F 2 F 3 F 4 Variable AOPT TSIZE ERODS SOFT Type F F F F Card 4 Variable 1 XP Type F 2 YP F 3 ZP F 4 A1 F F 5 FS F 5 A2 F F 6 6 A3 F F 7 F 8 7 8 PRCA PRCB F Card 5 Variable 1 V1 Type F Card 6 1 2 V2 F 2 3 V3 F 3 4 D1 F 4 5 D2 F 5 6 D3 F 6 7 8 BETA F 7 8 Variable E11C E11T E22C E22T GMS Type F F F F F 2 XT F 2 3 YC F 3 4 YT F 4 5 SC F 5 6 7 8 6 7 8 Card 7 Variable 1 XC Type F Card 8 Variable Type 1 K F Viscoelastic Cards. Up to 6 cards may be input. A keyword card (with a “*” in column 1) terminates this input if less than 6 cards are used. Optional Variable Type 1 GI F 2 3 4 5 6 7 8 BETAI *MAT_RATE_SENSITIVE_COMPOSITE_FABRIC DESCRIPTION MID RO EA EB (EC) PRBA PRCA PRCB TAU1 Material identification. A unique number or label not exceeding 8 characters must be specified. Mass density Ea, Young’s modulus - longitudinal direction Eb, Young’s modulus - transverse direction Ec, Young’s modulus - normal direction (not used) ba, Poisson’s ratio ba ca, Poisson’s ratio ca, can be defined in card 4, col. 7, default = PRBA cb, Poisson’s ratio cb, can be defined in card 4, col. 8, default = PRBA τ1, stress limit of the first slightly nonlinear part of the shear stress versus shear strain curve. The values τ1 and γ1 are used to define a curve of shear stress versus shear strain. These values are input if FS, defined below, is set to a value of -1. GAMMA1 γ1, strain limit of the first slightly nonlinear part of the shear stress versus shear strain curve. GAB GBC GCA SLIMT1 SLIMC1 SLIMT2 SLIMC2 Gab, shear modulus ab Gbc, shear modulus bc Gca, shear modulus ca Factor to determine the minimum stress limit after stress maximum (fiber tension). Factor to determine the minimum stress limit after stress maximum (fiber compression). Factor to determine the minimum stress limit after stress maximum (matrix tension). Factor to determine the minimum stress limit after stress maximum (matrix compression). VARIABLE DESCRIPTION SLIMS AOPT Factor to determine the minimum stress limit after stress maximum (shear). Material axes option : EQ.0.0: locally orthotropic with material axes determined by element nodes 1, 2, and 4, as with *DEFINE_COORDI- NATE_NODES, and then rotated about the shell ele- ment normal by the angle BETA. EQ.2.0: globally orthotropic with material axes determined by vectors defined below, as with *DEFINE_COORDI- NATE_VECTOR. EQ.3.0: locally orthotropic material axes determined by rotating the material axes about the element normal by an angle (BETA) from a line in the plane of the element defined by the cross product of the vector v with the element normal. LT.0.0: the absolute value of AOPT is a coordinate system ID number (CID on *DEFINE_COORDINATE_NODES, *DEFINE_COORDINATE_SYSTEM or *DEFINE_CO- ORDINATE_VECTOR). Available in R3 version of 971 and later. TSIZE Time step for automatic element deletion. ERODS Maximum effective strain for element layer failure. A value of unity would equal 100% strain. SOFT Softening reduction factor for strength in the crashfront. FS Failure surface type: EQ.1.0: smooth failure surface with a quadratic criterion for both the fiber (a) and transverse (b) directions. This option can be used with complete laminates and fab- rics. EQ.0.0: smooth failure surface in the transverse (b) direction with a limiting value in the fiber (a) direction. This model is appropriate for unidirectional (UD) layered composites only. EQ.-1: faceted failure surface. When the strength values are reached then damage evolves in tension and compres- *MAT_RATE_SENSITIVE_COMPOSITE_FABRIC DESCRIPTION sion for both the fiber and transverse direction. Shear behavior is also considered. This option can be used with complete laminates and fabrics. XP, YP, ZP Define coordinates of point p for AOPT = 1. A1, A2, A3 Define components of vector a for AOPT = 2. V1, V2, V3 Define components of vector v for AOPT = 3. D1, D2, D3 Define components of vector d for AOPT = 2. BETA E11C E11T E22C E22T GMS XC XT YC YT SC K GI Material angle in degrees for AOPT = 0 and 3, may be overridden on the element card, see *ELEMENT_SHELL_BETA. Strain at longitudinal compressive strength, a-axis. Strain at longitudinal tensile strength, a-axis. Strain at transverse compressive strength, b-axis. Strain at transverse tensile strength, b-axis. Strain at shear strength, ab plane. Longitudinal compressive strength Longitudinal tensile strength, see below. Transverse compressive strength, b-axis, see below. Transverse tensile strength, b-axis, see below. Shear strength, ab plane. Optional bulk modulus for the viscoelastic material. If nonzero a Kelvin type behavior will be obtained. Generally, K is set to zero. Optional shear relaxation modulus for the ith term BETAI Optional shear decay constant for the ith term Remarks: See the remark for material type 58, *MAT_LAMINATED_COMPOSITE_FABRIC, for the treatment of the composite material. Rate effects are taken into account through a Maxwell model using linear viscoelasticity by a convolution integral of the form: 𝜎𝑖𝑗 = ∫ 𝑔𝑖𝑗𝑘𝑙(𝑡 − 𝜏) ∂𝜀𝑘𝑙 ∂𝜏 𝑑𝜏 where 𝑔𝑖𝑗𝑘𝑙(𝑡−𝜏) is the relaxation functions for the different stress measures. This stress is added to the stress tensor determined from the strain energy functional. Since we wish to include only simple rate effects, the relaxation function is represented by six terms from the Prony series: 𝑔(𝑡) = ∑ 𝐺𝑚𝑒−𝛽𝑚𝑡 𝑚=1 We characterize this in the input by the shear moduli, 𝐺𝑖, and decay constants, 𝛽𝑖. An arbitrary number of terms, not exceeding 6, may be used when applying the viscoelastic model. The composite failure is not directly affected by the presence of the viscous stress tensor. *MAT_CSCM This is material type 159. This is a smooth or continuous surface cap model and is available for solid elements in LS-DYNA. The user has the option of inputting his own material properties (<BLANK> option), or requesting default material properties for normal strength concrete (CONCRETE). Available options include: <BLANK> CONCRETE Card 1 1 2 3 4 5 6 7 8 Variable MID RO NPLOT INCRE IRATE ERODE RECOV ITRETRC F 2 I 3 F 4 I 5 F 6 F 7 I 8 Type A8 Card 2 1 Variable PRED Type F Card 3 for CONCRETE keyword option. Card 3 1 2 3 4 5 6 7 8 Variable FPC DAGG UNITS Type F F The remaining cards are read when the keyword option is left blank. They are not read in when CONCRETE keyword option is active. Card 3 Variable Type 1 G F Card 4 1 2 K F 2 3 4 5 6 ALPHA THETA LAMDA BETA F 3 F 4 F 5 F 6 7 NH F 7 8 CH F 8 Variable ALPHA1 THETA1 LAMDA1 BETA1 ALPHA2 THETA2 LAMDA2 BETA2 Type F F Card 5 Variable Type Card 6 Variable Type 1 R F 1 B F Card 7 1 2 X0 F 2 GFC F 2 F 3 W F 3 D F 3 Variable ETA0C NC ETA0T Type F F F F F 4 D1 F 4 5 D2 F 5 F 6 F 7 F 8 6 7 8 GFT GFS PWRC PWRT PMOD F 4 NT F F 5 F 6 F 7 F 8 OVERC OVERT SRATE REPOW F F F MID *MAT_CSCM DESCRIPTION Material identification. A unique number or label not exceeding 8 characters must be specified. RO Mass density. NPLOT Controls what is written as component 7 to the d3plot database. LS-Prepost always blindly labels this component as effective plastic strain: EQ.1: Maximum of brittle and ductile damage (default). EQ.2: Maximum of brittle and ductile damage, with recovery of brittle damage. EQ.3: Brittle damage. EQ.4: Ductile damage. EQ.5: κ (intersection of cap with shear surface). EQ.6: X0 (intersection of cap with pressure axis). EQ.7: 𝜀v p (plastic volume strain). INCRE Maximum strain increment for subincrementation. If left blank, a default value is set during initialization based upon the shear strength and stiffness. IRATE Rate effects options: EQ.0: Rate effects model turned off (default). EQ.1: Rate effects model turned on. ERODE Elements erode when damage exceeds 0.99 and the maximum principal strain exceeds ERODE-1.0. For erosion that is independent of strain, set ERODE equal to 1.0. Erosion does not occur if ERODE is less than 1.0. RECOV *MAT_159 DESCRIPTION The modulus is recovered in compression when RECOV is equal to 0 (default). The modulus remains at the brittle damage level when RECOV is equal to 1. Partial recovery is modeled for values of RECOV between 0 and 1. Two options are available: EQ.1: Input a value between 0 and 1. Recovery is based upon the sign of the pressure invariant only. EQ.2: Input a value between 10 and 11. Recovery is based upon the sign of both the pressure and volumetric strain. In this case, RECOV = RECOV-10, and a flag is set to request the volumetric strain check. IRETRC Cap retraction option: EQ.0: Cap does not retract (default). EQ.1: Cap retracts. PRED Pre-existing damage (0 ≤ PreD < 1). If left blank, the default is zero (no pre-existing damage). Define for the CONCRETE option only: VARIABLE FPC DESCRIPTION Unconfined compression strength, f 'C. Material parameters are internally fit to data for unconfined compression strengths between about 20 and 58 Mpa (2,901 to 8,412 psi), with emphasis on the midrange between 28 and 48 MPa (4,061 and 6,962 psi). If left blank, default for FPC is 30 MPa. DAGG Maximum aggregate size, Dagg. Softening is fit to data for aggregate sizes between 8 and 32 mm (0.3 and 1.3 inches). If left blank, default for DAGG is 19 mm (3/4 inch). UNITS Units options: EQ.0: GPa, mm, msec, Kg/mm3, kN EQ.1: MPa, mm, msec, g/mm3, N EQ.2: MPa, mm, sec, Mg/mm3, N EQ.3: Psi, inch, sec, lbf-s2/inch4, lbf EQ.4: Pa, m, sec, kg/m3, N *MAT_CSCM VARIABLE DESCRIPTION G K ALPHA THETA Shear modulus. Bulk modulus. Tri-axial compression surface constant term, α. Tri-axial compression surface linear term, θ. LAMDA Tri-axial compression surface nonlinear term, λ. BETA Tri-axial compression surface exponent, β. ALPHA1 Torsion surface constant term, α1. THETA1 Torsion surface linear term, θ1. LAMDA1 Torsion surface nonlinear term, λ1. BETA1 Torsion surface exponent, β1. ALPHA2 Tri-axial extension surface constant term, α2. THETA2 Tri-axial extension surface linear term, θ2. LAMDA2 Tri-axial extension surface nonlinear term, λ2. BETA2 Tri-axial extension surface exponent, β2. NH CH R X0 W D1 D2 B Hardening initiation, NH. Hardening rate, CH. Cap aspect ratio, R. Cap initial location, X0. Maximum plastic volume compaction, W. Linear shape parameter, D1. Quadratic shape parameter, D2. Ductile shape softening parameter, B. VARIABLE GFC D GFT GFS PWRC PWRT DESCRIPTION Fracture energy in uniaxial stress Gfc. Brittle shape softening parameter, D. Fracture energy in uniaxial tension, Gft. Fracture energy in pure shear stress, Gfs. Shear-to-compression transition parameter. Shear-to-tension transition parameter. PMOD Modify moderate pressure softening parameter. ETA0C Rate effects parameter for uniaxial compressive stress, η0c. NC Rate effects power for uniaxial compressive stress, NC. ETA0T Rate effects parameter for uniaxial tensile stress, η0t. NT Rate effects power for uniaxial tensile stress, Nt. OVERC Maximum overstress allowed in compression. OVERT Maximum overstress allowed in tension. SRATE Ratio of effective shear stress to tensile stress fluidity parameters. REPOW Power which increases fracture energy with rate effects. Model Formulation and Input Parameters: Shear Surface Smooth Intersection Cap Pressure Figure M159-1. General shape of concrete model yield surface in two dimensions. This is a cap model with a smooth intersection between the shear yield surface and hardening cap, as shown in Figure M159-1. The initial damage surface coincides with the yield surface. Rate effects are modeled with viscoplasticity. For a complete theoretical description, with references and example problems see [Murray 2007] and [Murray, Abu-Odeh and Bligh 2007]. Stress Invariants. The yield surface is formulated in terms of three stress invariants: 𝐽1 is ′ is the second invariant of the deviatoric stress the first invariant of the stress tensor, 𝐽2 ′ is the third invariant of the deviatoric stress tensor. The invariants are tensor, and 𝐽3 defined in terms of the deviatoric stress tensor, Sij and pressure, P, as follows: 𝐽1 = 3P ′ = 𝐽2 ′ = 𝐽3 SijSij SijSjkSki Plasticity Surface. The three invariant yield function is based on these three invariants, and the cap hardening parameter, κ, as follows: ′ , 𝜅) = 𝐽2 Here 𝐹f is the shear failure surface, 𝐹c is the hardening cap, and ℜ is the Rubin three- invariant reduction factor. The cap hardening parameter 𝜅 is the value of the pressure invariant at the intersection of the cap and shear surfaces. ′ − ℜ2𝐹𝑓 𝑓 (𝐽1, 𝐽2 2𝐹𝑐 ′ , 𝐽3 Trial elastic stress invariants are temporarily updated via the trial elastic stress tensor, ′𝑇. Elastic stress states are modeled when 𝝈𝑇. These are denoted J1 ′𝑇, 𝜅𝑇) ≤ 𝑓 (𝐽1 ′𝑇, 𝜅𝑇) ≤ 0. Elastic-plastic stress states are modeled when 𝑓 (𝐽1 ′𝑇, and J3 𝑇, J2 ′𝑇, 𝐽3 ′𝑇, 𝐽3 𝑇, 𝐽2 𝑇, 𝐽2 0. In this case, the plasticity algorithm returns the stress state to the yield surface such ′𝑃, 𝜅𝑃) = 0. This is accomplished by enforcing the plastic consistency that 𝑓 (𝐽1 condition with associated flow. ′𝑃, 𝐽3 𝑃, 𝐽2 Shear Failure Surface. The strength of concrete is modeled by the shear surface in the tensile and low confining pressure regimes: 𝐹𝑓 (J1) = 𝛼 − 𝜆 exp−𝛽 J1 + 𝜃𝐽1 Here the values of 𝛼, 𝛽, 𝜆, and 𝜃 are selected by fitting the model surface to strength measurements from triaxial compression (TXC) tests conducted on plain concrete cylinders. ′ (principal stress Rubin Scaling Function. Concrete fails at lower values of √3𝐽2 difference) for triaxial extension (TXE) and torsion (TOR) tests than it does for TXC tests conducted at the same pressure. The Rubin scaling function ℜ determines the strength of concrete for any state of stress relative to the strength for TXC, via ℜFf. Strength in torsion is modeled as Q1Ff . Strength in TXE is modeled as Q2Ff, where: 𝑄1 = 𝛼1 − 𝜆1exp−𝛽1J1 + 𝜃1𝐽1 𝑄2 = 𝛼2 − 𝜆2exp−𝛽2J1 + 𝜃2𝐽1 Cap Hardening Surface. The strength of concrete is modeled by a combination of the cap and shear surfaces in the low to high confining pressure regimes. The cap is used to model plastic volume change related to pore collapse (although the pores are not explicitly modeled). The isotropic hardening cap is a two-part function that is either unity or an ellipse: 𝐹𝑐( 𝐽1, 𝜅 ) = 1 − [𝐽1 − 𝐿 (𝜅)][ |𝐽1 − 𝐿(𝜅)| + 𝐽1 − 𝐿(𝜅) ] 2 [𝑋(𝜅) − 𝐿 (𝜅)] 2 where 𝐿(𝜅) is defined as: 𝐿(𝜅) = { if 𝜅 > 𝜅0 𝜅0 otherwise The equation for 𝐹𝑐 is equal to unity for 𝐽1 ≤ 𝐿(𝜅). It describes the ellipse for J1 > L(κ). The intersection of the shear surface and the cap is at J1 = κ. κ0 is the value of J1 at the initial intersection of the cap and shear surfaces before hardening is engaged (before the cap moves). The equation for L(κ) restrains the cap from retracting past its initial location at κ0. The intersection of the cap with the J1 axis is at J1 = X(κ). This intersection depends upon the cap ellipticity ratio R, where R is the ratio of its major to minor axes: 𝑋(𝜅) = 𝐿(𝜅) + R𝐹𝑓 [𝐿(𝜅)] The cap expands (X(κ) The cap moves to simulate plastic volume change. and κ increase) to simulate plastic volume compaction. The cap contracts (X(κ) and κ decrease) to simulate plastic volume expansion, called dilation. The motion (expansion and contraction) of the cap is based upon the hardening rule: 𝑝 = 𝑊[1 − 𝑒−𝐷1(𝑋−𝑋0)−𝐷2(𝑋−𝑋0)2 𝜀𝑣 ] p the plastic volume strain, W is the maximum plastic volume strain, and D1 and Here 𝜀v D2 are model input parameters. X0 is the initial location of the cap when κ = κ0. The five input parameters (X0, W, D1, D2, and R) are obtained from fits to the pressure- volumetric strain curves in isotropic compression and uniaxial strain. X0 determines the pressure at which compaction initiates in isotropic compression. R, combined with X0, determines the pressure at which compaction initiates in uniaxial strain. D1, and D2 determine the shape of the pressure-volumetric strain curves. W determines the maximum plastic volume compaction. Shear Hardening Surface. In unconfined compression, the stress-strain behavior of concrete exhibits nonlinearity and dilation prior to the peak. Such behavior is be modeled with an initial shear yield surface, NHFf , which hardens until it coincides with the ultimate shear yield surface, Ff. Two input parameters are required. One parameter, NH, initiates hardening by setting the location of the initial yield surface. A second parameter, CH, determines the rate of hardening (amount of nonlinearity). Damage. Concrete exhibits softening in the tensile and low to moderate compressive regimes. d = (1 − 𝑑)𝜎ij 𝜎ij vp A scalar damage parameter, d, transforms the viscoplastic stress tensor without damage, denoted σvp, into the stress tensor with damage, denoted σd. Damage accumulation is based upon two distinct formulations, which we call brittle damage and ductile damage. The initial damage threshold is coincident with the shear plasticity surface, so the threshold does not have to be specified by the user. Ductile Damage. Ductile damage accumulates when the pressure (P) is compressive and an energy-type term, τc, exceeds the damage threshold, τ0c. Ductile damage accumulation depends upon the total strain components, εij, as follows: The stress components σij are the elasto-plastic stresses (with kinematic hardening) calculated before application of damage and rate effects. 𝜏c = √ 𝜎𝑖𝑗𝜀𝑖𝑗 Brittle Damage. Brittle damage accumulates when the pressure is tensile and an energy- type term, τt, exceeds the damage threshold, τ0t. Brittle damage accumulation depends upon the maximum principal strain, ε max, as follows: Softening Function. As damage accumulates, the damage parameter d increases from an initial value of zero, towards a maximum value of one, via the following formulations: 𝜏t = √𝐸 𝜀 max Brittle Damage: 𝑑(𝜏𝑡) = Ductile Damage: 𝑑(𝜏𝑐) = 0.999 𝑑max 1 + 𝐷 [ 1 + 𝐷 𝑒−𝐶(𝜏𝑡−𝜏0𝑡) − 1] 1 + 𝐵𝑒−𝐴(𝜏𝑐−𝜏0𝑐) − 1] 1 + 𝐵 [ The damage parameter that is applied to the six stresses is equal to the current maximum of the brittle or ductile damage parameter. The parameters A and B or C and D set the shape of the softening curve plotted as stress-displacement or stress-strain. The parameter dmax is the maximum damage level that can be attained. It is calculated internally calculated and is less than one at moderate confining pressures. The compressive softening parameter, A, may also be reduced with confinement, using the input parameter pmod, as follows: 𝐴 = 𝐴(𝑑max + 0.001)pmod Regulating Mesh Size Sensitivity. The concrete model maintains constant fracture energy, regardless of element size. The fracture energy is defined here as the area under the stress-displacement curve from peak strength to zero strength. This is done by internally formulating the softening parameters A and C in terms of the element length, l (cube root of the element volume), the fracture energy, Gf, the initial damage threshold, τ0t or τ0c, and the softening shape parameters, D or B. The fracture energy is calculated from up to five user-specified input parameters: GFC, GFS, GFT, PWRC, and PWRT. The user specifies three distinct fracture energy values. These are the fracture energy in uniaxial tensile stress, GFT, pure shear stress, GFS, and uniaxial compressive stress, GFC. The model internally selects the fracture energy from equations which interpolate between the three fracture energy values as a function of the stress state (expressed via two stress invariants). The interpolation equations depend upon the user-specified input powers PWRC and PWRT, as follows. Tensile Pressure: 𝐺𝑓 = GFS + Compressive Pressure: 𝐺𝑓 = GFS + 𝑘𝑡 ⏞⏞⏞⏞⏞⏞⏞ PWRT ⎜⎜⎜⎛ −𝐽1 ⎟⎟⎟⎞ ′ √3𝐽2 ⎠ ⎝ 𝑘𝑐 ⏞⏞⏞⏞⏞⏞⏞ PWRC ⎜⎜⎜⎛ 𝐽1 ⎟⎟⎟⎞ ′ √3𝐽2 ⎠ ⎝ [GFT − GFS] [GFC − GFS] The internal parameters 𝑘𝑐 and 𝑘𝑡 are restricted to the interval [0,1]. Element Erosion. An element losses all strength and stiffness as d→1. To prevent computational difficulties with very low stiffness, element erosion is available as a user option. An element erodes when d > 0.99 and the maximum principal strain is greater than a user supplied input value, ERODE-1.0. Viscoplastic Rate Effects. At each time step, the viscoplastic algorithm interpolates p, to between the elastic trial stress, 𝜎𝑖j set the viscoplastic stress (with rate effects), 𝜎𝑖j T, and the inviscid stress (without rate effects), 𝜎𝑖j vp: vp = (1 − 𝛾)σij σij p T + 𝛾σij where, 𝛾 = Δt/𝜂 1 + Δt/𝜂 . This interpolation depends upon the effective fluidity coefficient, η, and the time step, Δt. The effective fluidity coefficient is internally calculated from five user-supplied input parameters and interpolation equations: Tensile Pressure: 𝜂 = 𝜂𝑠 + Compressive Pressure: 𝜂 = 𝜂𝑠 + where, PWRT ⎟⎟⎟⎞ ⎠ PWRC ⎜⎜⎜⎛ −𝐽1 ′ √3𝐽2 ⎝ ⎜⎜⎜⎛ 𝐽1 ′ √3𝐽2 ⎝ ⎟⎟⎟⎞ ⎠ [𝜂𝑡 − 𝜂𝑠] [𝜂𝑐 − 𝜂𝑠] 𝜂𝑠 = SRATE × 𝜂𝑡 𝜂𝑡 = ETA0T 𝜖 ̇NT 𝜂𝑐 = ETA0C 𝜖 ̇NC The input parameters are ΕΤΑ0Τ and NT for fitting uniaxial tensile stress data, ΕΤΑ0Χ and NC for fitting the uniaxial compressive stress data, and SRATE for fitting shear stress data. The effective strain rate is 𝜀̇. This viscoplastic model may predict substantial rate effects at high strain rates (𝜀̇ > 100). To limit rate effects at high strain rates, the user may input overstress limits in tension OVERT and compression OVERC. These input parameters limit calculation of the fluidity parameter, as follows: if 𝐸𝜖 ̇𝜂 > OVER, then 𝜂 = 𝐸𝜖 ̇ where m = OVERT when the pressure is tensile, and m = OVERC when the pressure is compressive. The user has the option of increasing the fracture energy as a function of effective strain rate via the REPOW input parameter, as follows: Gf rate = Gf (1 + Eε̇η f′ rate is the fracture energy enhanced by rate effects, and f′ is the yield strength Here Gf before application of rate effects (which is calculated internally by the model). The term in brackets is greater than, or equal to one, and is the approximate ratio of the dynamic to static strength. ) REPOW *MAT_ALE_INCOMPRESSIBLE This is Material Type 160. This card allows to solve incompressible flows with the ALE solver. It should be used with the element formulation 6 and 12 in *SECTION_SOLID (elform = 6 or 12). A projection method enforces the incompressibility condition. 5 6 7 8 Card 1 1 Variable MID Type I 2 RO F 3 PC F 4 MU F Default none none 0.0 0.0 Card 2 1 2 3 4 5 6 7 8 Variable TOL DTOUT NCG METH Type F F I I Default 1e-8 1e10 50 -7 VARIABLE DESCRIPTION MID RO PC MU TOL Material ID. A unique number or label not exceeding 8 charaters must be specified. Material ID is referenced in the *PART card and must be unique Material density Pressure cutoff (< or = 0.0) Dynamic viscosity coefficient Tolerance for the convergence of the conjugate gradient DTOUT Time interval between screen outputs NCG Maximum number of loops in the conjugate gradient VARIABLE DESCRIPTION METH Conjugate gradient methods: EQ.-6: solves the poisson equation for the pressure EQ.-7: solves the poisson equation for the pressure increment *MAT_COMPOSITE_MSC_{OPTION} Available options include: <BLANK> DMG These are Material Types 161 and 162. These models may be used to model the progressive failure analysis for composite materials consisting of unidirectional and woven fabric layers. The progressive layer failure criteria have been established by adopting the methodology developed by Hashin [1980] with a generalization to include the effect of highly constrained pressure on composite failure. These failure models can be used to effectively simulate fiber failure, matrix damage, and delamination behavior under all conditions - opening, closure, and sliding of failure surfaces. The model with DMG option (material 162) is a generalization of the basic layer failure model of Material 161 by adopting the damage mechanics approach for characterizing the softening behavior after damage initiation. These models require an additional license from Materials Sciences Corporation, which developed and supports these models. Card 1 1 Variable MID Type A8 Card 2 1 2 RO F 2 3 EA F 3 4 EB F 4 5 EC F 5 Variable GAB GBC GCA AOPT MACF Type F F F F I Card 3 Variable 1 XP Type F 2 YP F 3 ZP F 4 A1 F 5 A2 F 6 7 8 PRBA PRCA PRCB F 7 F 8 7 8 F 6 6 A3 Card 4 Variable 1 V1 Type F Card 5 1 2 V2 F 2 3 V3 F 3 4 D1 F 4 5 D2 F 5 6 D3 F 6 7 8 BETA F 7 8 Variable SAT SAC SBT SBC SCT SFC SFS SAB Type F Card 6 1 F 2 F 3 F 4 F 5 F 6 F 7 Variable SBC SCA SFFC AMODEL PHIC E_LIMT S_DELM Type F Card 7 1 F 2 F 3 F 4 F 5 F 6 F 7 F 8 8 Variable OMGMX ECRSH EEXPN CERATE1 AM1 Type F F F F F Failure Card. Additional card for DMG keyword option. Card 8 1 2 3 4 5 6 7 8 Variable AM2 AM3 AM4 CERATE2 CERATE3 CERATE4 Type F F F F F F VARIABLE MID LS-DYNA R10.0 DESCRIPTION Material identification. A unique number or label not exceeding 8 RO EA EB EC PRBA PRCA PRCB GAB GBC GCA Mass density Ea, Young’s modulus - longitudinal direction Eb, Young’s modulus - transverse direction Ec, Young’s modulus - through thickness direction ba, Poisson’s ratio ba ca, Poisson’s ratio ca cb, Poisson’s ratio cb Gab, shear modulus ab Gbc, shear modulus bc Gca, shear modulus ca AOPT Material axes option, see Figure 2.1: EQ.0.0: locally orthotropic with material axes determined by element nodes as shown in Figure 2.1. Nodes 1, 2, and 4 of an element are identical to the Nodes used for the definition of a coordinate system by *DEFINE_COOR- DINATE_NODES. EQ.1.0: locally orthotropic with material axes determined by a point in space and the global location of the element center, to define the a-direction. EQ.2.0: globally orthotropic with material axes determined by vectors defined below, as with *DEFINE_COORDI- NATE_VECTOR. EQ.3.0: locally orthotropic material axes determined by rotating the material axes about the element normal by an angle, BETA, from a line in the plane of the element defined by the cross product of the vector v with the element normal. The plane of a solid element is the midsurface between the inner surface and outer surface defined by the first four nodes and the last four nodes of the connectivity of the element, respectively. EQ.4.0: locally orthotropic in cylindrical coordinate system with the material axes determined by a vector v, and an originating point, p, which define the centerline ax- is. This option is for solid elements only. LT.0.0: the absolute value of AOPT is a coordinate system ID number (CID on *DEFINE_COORDINATE_NODES, *DEFINE_COORDINATE_SYSTEM or *DEFINE_CO- ORDINATE_VECTOR). Available in R3 version of 971 and later. MACF Material axes change flag: EQ.1: No change, default, EQ.2: switch material axes a and b, EQ.3: switch material axes a and c, EQ.4: switch material axes b and c. XP, YP, ZP Define coordinates of point p for AOPT = 1 and 4. A1, A2, A3 Define components of vector a for AOPT = 2. V1, V2, V3 Define components of vector v for AOPT = 3 and 4. D1, D2, D3 Define components of vector d for AOPT = 2. BETA Layer in-plane rotational angle in degrees. SAT SAC SBT SBC SCT SFC SFS SAB SBC SCA Longitudinal tensile strength Longitudinal compressive strength Transverse tensile strength Transverse compressive strength Through thickness tensile strength Crush strength Fiber mode shear strength Matrix mode shear strength, ab plane, see below. Matrix mode shear strength, bc plane, see below. Matrix mode shear strength, ca plane, see below. SFFC Scale factor for residual compressive strength AMODEL Material models: EQ.1.0: Unidirectional layer model EQ.2.0: Fabric layer model PHIC Coulomb friction angle for matrix and delamination failure, < 90 E_LIMT Element eroding axial strain S_DELM Scale factor for delamination criterion OMGMX Limit damage parameter for elastic modulus reduction ECRSH Limit compressive volume strain for element eroding EEXPN Limit tensile volume strain for element eroding CERATE1 Coefficient for strain rate dependent strength properties AM1 AM2 AM3 AM4 Coefficient for strain rate softening property for fiber damage in a direction. Coefficient for strain rate softening property for fiber damage in b direction. Coefficient for strain rate softening property for fiber crush and punch shear damage. Coefficient for strain rate softening property for matrix and delamination damage. CERATE2 Coefficient for strain rate dependent axial moduli. CERATE3 Coefficient for strain rate dependent shear moduli. CERATE4 Coefficient for strain rate dependent transverse moduli. Material Models: in The unidirectional and fabric layer failure criteria and the associated property degradation models for material 161 are described as follows. All the failure criteria are expressed stresses (𝜎𝑎, 𝜎𝑏, 𝜎𝑐, 𝜏𝑎𝑏, 𝜏𝑏𝑐, 𝜏𝑐𝑎) and the associated elastic moduli are (𝐸𝑎, 𝐸𝑏, 𝐸𝑐, 𝐺𝑎𝑏, 𝐺𝑏𝑐, 𝐺𝑐𝑎). Note that for the unidirectional model, a, b and c denote the fiber, in-plane transverse and out-of-plane directions, respectively, while for the fabric model, a, b and c denote the in-plane fill, in-plane warp and out-of-plane directions, respectively. components based on ply terms of stress level Unidirectional lamina model: Three criteria are used for fiber failure, one in tension/shear, one in compression and another one in crush under pressure. They are chosen in terms of quadratic stress forms as follows: Tensile/shear fiber mode: 𝑓1 = ( ) 〈𝜎𝑎〉 𝑆𝑎𝑇 + ( 2 + 𝜏𝑐𝑎 𝜏𝑎𝑏 𝑆𝐹𝑆 ) − 1 = 0 Compression fiber mode: Crush mode: 𝑓2 = ( ) ′〉 〈𝜎𝑎 𝑆𝑎𝐶 − 1 = 0, 𝜎𝑎 ′ = −𝜎𝑎 + ⟨− 𝜎𝑏 + 𝜎𝑐 ⟩ 𝑓3 = ( ⟨𝑝⟩ 𝑆𝐹𝐶 ) − 1 = 0, 𝑝 = − 𝜎𝑎 + 𝜎𝑏 + 𝜎𝑐 ⟩ are Macaulay brackets, 𝑆𝑎𝑇 and 𝑆𝑎𝐶 are the tensile and compressive strengths where ⟨ in the fiber direction, and 𝑆𝐹𝑆 and 𝑆𝐹𝐶 are the layer strengths associated with the fiber shear and crush failure, respectively. Matrix mode failures must occur without fiber failure, and hence they will be on planes parallel to fibers. For simplicity, only two failure planes are considered: one is perpendicular to the planes of layering and the other one is parallel to them. The matrix failure criteria for the failure plane perpendicular and parallel to the layering planes, respectively, have the forms: Perpendicular matrix mode: 𝑓4 = ( ) ⟨𝜎𝑏⟩ 𝑆𝑏𝑇 + ( 𝜏𝑏𝑐 ′ ) 𝑆𝑏𝑐 + ( ) 𝜏𝑎𝑏 𝑆𝑎𝑏 − 1 = 0 Parallel matrix mode (Delamination): ( 𝑓5 = 𝑆2 𝜏𝑏𝑐 " 𝑆𝑏𝑐 where SbT is the transverse tensile strength. Based on the Coulomb-Mohr theory, the shear strengths for the transverse shear failure and the two axial shear failure modes are assumed to be the forms, ⟨𝜎𝑐⟩ 𝑆𝑏𝑇 − 1 = 0 𝜏𝑐𝑎 𝑆𝑐𝑎 + ( + ( ) ) ) }⎫ ⎭}⎬ {⎧ ⎩{⎨ 𝑆𝑎𝑏 = 𝑆𝑎𝑏 ′ = 𝑆𝑏𝑐 𝑆𝑏𝑐 𝑆𝑐𝑎 = 𝑆𝑐𝑎 (0) + tan(𝜑)⟨−𝜎𝑏⟩ (0) + tan(𝜑)⟨−𝜎𝑏⟩ (0) + tan(𝜑)⟨−𝜎𝑐⟩ " = 𝑆𝑏𝑐 𝑆𝑏𝑐 (0) + tan(𝜑)⟨−𝜎𝑐⟩ where ϕ is a material constant as tan(𝜑) is similar to the coefficient of friction, and 𝑆𝑎𝑏 (0)are the shear strength values of the corresponding tensile modes. (0)and 𝑆𝑏𝑐 𝑆𝑐𝑎 (0), Failure predicted by the criterion of f4 can be referred to as transverse matrix failure, while the matrix failure predicted by f5, which is parallel to the layer, can be referred as the delamination mode when it occurs within the elements that are adjacent to the ply interface. Note that a scale factor S is introduced to provide better correlation of delamination area with experiments. The scale factor S can be determined by fitting the analytical prediction to experimental data for the delamination area. When fiber failure in tension/shear mode is predicted in a layer by f1, the load carrying capacity of that layer is completely eliminated. All the stress components are reduced to zero instantaneously (100 time steps to avoid numerical instability). For compressive fiber failure, the layer is assumed to carry a residual axial load, while the transverse load carrying capacity is reduced to zero. When the fiber compressive failure mode is reached due to f2, the axial layer compressive strength stress is assumed to reduce to a residual value 𝑆𝑅𝐶 (=SFFC × 𝑆𝐴𝐶). The axial stress is then assumed to remain constant, i.e., 𝜎𝑎 = −𝑆𝑅𝐶, for continuous compressive loading, while the subsequent unloading curve follows a reduced axial modulus to zero axial stress and strain state. When the fiber crush failure occurs, the material is assumed to behave elastically for compressive pressure, p > 0, and to carry no load for tensile pressure, p < 0. (0)and 𝑆𝑏𝑐 When a matrix failure (delamination) in the a-b plane is predicted, the strength values (0) are set to zero. This results in reducing the stress components 𝜎𝑐, 𝜏𝑏𝑐 for 𝑆𝑐𝑎 and 𝜏𝑐𝑎 to the fractured material strength surface. For tensile mode, 𝜎𝑐 > 0, these stress components are reduced to zero. For compressive mode, 𝜎𝑐 < 0, the normal stress 𝜎𝑐 is assumed to deform elastically for the closed matrix crack. Loading on the failure envelop, the shear stresses are assumed to ‘slide’ on the fractured strength surface (frictional shear stresses) like in an ideal plastic material, while the subsequent unloading shear stress-strain path follows reduced shear moduli to the zero shear stress and strain state for both 𝜏𝑏𝑐 and 𝜏𝑐𝑎 components. (0)and 𝑆𝑏𝑐 The post failure behavior for the matrix crack in the a-c plane due to f4 is modeled in the same fashion as that in the a-b plane as described above. In this case, when failure (0)are reduced to zero instantaneously. The post fracture response is occurs, 𝑆𝑎𝑏 (0)= 0. For tensile mode, then governed by failure criterion of f5 with 𝑆𝑎𝑏 𝜎𝑏 > 0, 𝜎𝑏, 𝜏𝑎𝑏 and 𝜏𝑏𝑐 are zero. For compressive mode, 𝜎𝑏 < 0, 𝜎𝑏 is assumed to be elastic, while 𝜏𝑎𝑏 and 𝜏𝑏𝑐 ‘slide’ on the fracture strength surface as in an ideal plastic material, and the unloading path follows reduced shear moduli to the zero shear stress and strain state. It should be noted that 𝜏𝑏𝑐 is governed by both the failure functions and should lie within or on each of these two strength surfaces. (0)= 0 and 𝑆𝑏𝑐 Fabric lamina model: The fiber failure criteria of Hashin for a unidirectional layer are generalized to characterize the fiber damage in terms of strain components for a plain weave layer. The fill and warp fiber tensile/shear failure are given by the quadratic interaction between the associated axial and shear stresses, i.e. 2 + 𝜏𝑐𝑎 2 ) 𝑆𝑎𝐹𝑆 2 ) 2 + 𝜏𝑏𝑐 𝑆𝑏𝐹𝑆 ⟨𝜎𝑏⟩ 𝑆𝑏𝑇 ⟨𝜎𝑎⟩ 𝑆𝑎𝑇 − 1 = 0 − 1 = 0 𝑓7 = ( 𝑓6 = ( (𝜏𝑎𝑏 (𝜏𝑎𝑏 ) + + ) where 𝑆𝑎𝑇and 𝑆𝑏𝑇 are the axial tensile strengths in the fill and warp directions, respectively, and 𝑆𝑎𝐹𝑆 and 𝑆𝑏𝐹𝑆 are the layer shear strengths due to fiber shear failure in the fill and warp directions. These failure criteria are applicable when the associated 𝜎𝑎 or 𝜎𝑏 is positive. It is assumed 𝑆𝑎𝐹𝑆= SFS, and 𝑆𝑏𝐹𝑆 = SFS × 𝑆𝑏𝑇 𝑆𝑎𝑇 . When 𝜎𝑎 or 𝜎𝑏is compressive, it is assumed that the in-plane compressive failure in both the fill and warp directions are given by the maximum stress criterion, i.e. 𝑓8 = [ ′⟩ ⟨𝜎𝑎 ] 𝑆𝑎𝐶 𝑓9 = [ ] ′⟩ ⟨𝜎𝑏 𝑆𝑏𝐶 − 1 = 0, 𝜎𝑎 ′ = −𝜎𝑎 + ⟨−𝜎𝑐⟩ − 1 = 0, 𝜎𝑏 ′ = −𝜎𝑏 + ⟨−𝜎𝑐⟩ where 𝑆𝑎𝐶and 𝑆𝑏𝐶 are the axial compressive strengths in the fill and warp directions, respectively. The crush failure under compressive pressure is 𝑓10 = ( ⟨𝑝⟩ 𝑆𝐹𝐶 ) − 1 = 0, 𝑝 = − 𝜎𝑎 + 𝜎𝑏 + 𝜎𝑐 A plain weave layer can fail under in-plane shear stress without the occurrence of fiber breakage. This in-plane matrix failure mode is given by 𝑓11 = ( 𝜏𝑎𝑏 𝑆𝑎𝑏 ) − 1 = 0 where 𝑆𝑎𝑏 is the layer shear strength due to matrix shear failure. Another failure mode, which is due to the quadratic interaction between the thickness stresses, is expected to be mainly a matrix failure. This through the thickness matrix failure criterion is 𝑓12 = 𝑆2 {( ⟨𝜎𝑐⟩ 𝑆𝑐𝑇 ) 2 + ( 𝜏𝑏𝑐 𝑆𝑏𝑐 ) + ( 𝜏𝑐𝑎 𝑆𝑐𝑎 ) } − 1 = 0 where 𝑆𝑐𝑇 is the through the thickness tensile strength, and 𝑆𝑏𝑐, and 𝑆𝑐𝑎 are the shear strengths assumed to depend on the compressive normal stress 𝜎𝑐, i.e., 𝑆𝑐𝑎 { 𝑆𝑏𝑐 } = { (0) 𝑆𝑐𝑎 (0)} + tan(𝜑)⟨−𝜎𝑐⟩ 𝑆𝑏𝑐 When failure predicted by this criterion occurs within elements that are adjacent to the ply interface, the failure plane is expected to be parallel to the layering planes, and, thus, can be referred to as the delamination mode. Note that a scale factor S is introduced to provide better correlation of delamination area with experiments. The scale factor S can be determined by fitting the analytical prediction to experimental data for the delamination area. Similar to the unidirectional model, when fiber tensile/shear failure is predicted in a layer by f6 or f7, the load carrying capacity of that layer in the associated direction is completely eliminated. For compressive fiber failure due to by f8 or f9, the layer is assumed to carry a residual axial load in the failed direction, while the load carrying capacity transverse to the failed direction is assumed unchanged. When the compressive axial stress in a layer reaches the compressive axial strength 𝑆𝑎𝐶 or 𝑆𝑏𝐶, the axial layer stress is assumed to be reduced to the residual strength 𝑆𝑎𝑅𝐶 or 𝑆𝑏𝑅𝐶 where 𝑆𝑎𝑅𝐶 = SFFC × 𝑆𝑎𝐶 and 𝑆𝑏𝑅𝐶 = SFFC × 𝑆𝑏𝐶. The axial stress is assumed to remain constant, i.e., 𝜎𝑎 = −𝑆𝑎𝐶𝑅 or 𝜎𝑏 = −𝑆𝑏𝐶𝑅, for continuous compressive loading, while the subsequent unloading curve follows a reduced axial modulus. When the fiber crush failure is occurred, the material is assumed to behave elastically for compressive pressure, p > 0, and to carry no load for tensile pressure, p < 0. When the in-plane matrix shear failure is predicted by f11 the axial load carrying capacity within a failed element is assumed unchanged, while the in-plane shear stress is assumed to be reduced to zero. For through the thickness matrix (delamination) failure given by equations f12, the in- plane load carrying capacity within the element is assumed to be elastic, while the (0), are set to zero. For tensile mode, (0) and 𝑆𝑏𝑐 strength values for the tensile mode, 𝑆𝑐𝑎 𝜎𝑐 > 0, the through the thickness stress components are reduced to zero. For compressive mode, 𝜎𝑐 < 0, 𝜎𝑐 is assumed to be elastic, while 𝜏𝑏𝑐 and 𝜏𝑐𝑎 ‘slide’ on the fracture strength surface as in an ideal plastic material, and the unloading path follows reduced shear moduli to the zero shear stress and strain state. The effect of strain-rate on the layer strength values of the fiber failure modes is modeled by the strain-rate dependent functions for the strength values {𝑆𝑅𝑇} as {𝑆𝑅𝑇 } = {𝑆0 } ( 1 + 𝐶rate1 ln ̇} {𝜀̅ 𝜀̇0 ) {𝑆𝑅𝑇} = ⎧𝑆𝑎𝑇 ⎫ } { } 𝑆𝑎𝐶 { } { } { 𝑆𝑏𝑇 ⎬ ⎨ 𝑆𝑏𝐶 } { } { 𝑆𝐹𝐶 } { } { 𝑆𝐹𝑆 ⎭ ⎩ , {𝜀̅ ̇} = ⎧ {{{{{ {{{{{ ⎨ ⎩ ∣𝜀̇𝑎∣ ∣𝜀̇𝑎∣ ∣𝜀̇𝑏∣ ∣𝜀̇𝑏∣ ∣𝜀̇𝑐∣ 2 ) 2 + 𝜀̇𝑏𝑐 (𝜀̇𝑐𝑎 1/2 ⎫ }}}}} }}}}} ⎬ ⎭ where Crate is the strain-rate constants, and {𝑆0 }are the strength values of {𝑆𝑅𝑇 } at the reference strain-rate 𝜀̇0. Damage model: The damage model is a generalization of the layer failure model of Material 161 by adopting the MLT damage mechanics approach, Matzenmiller et al. [1995], for characterizing the softening behavior after damage initiation. Complete model description is given in Yen [2002]. The damage functions, which are expressed in terms of ply level engineering strains, are converted from the above failure criteria of fiber and matrix failure modes by neglecting the Poisson’s effect. Elastic moduli reduction is expressed in terms of the associated damage parameters 𝜛𝑖: ′ = (1 − 𝜛𝑖)𝐸𝑖 𝐸𝑖 𝜛𝑖 = 1 − exp (− 𝑚𝑖 𝑟𝑖 𝑚𝑖 ) , 𝑟𝑖 ≥ 0, 𝑖 = 1, . . . ,6, ′ are the reduced elastic moduli, 𝑟𝑖 are the where 𝐸𝑖 are the initial elastic moduli, 𝐸𝑖 damage thresholds computed from the associated damage functions for fiber damage, matrix damage and delamination, and mi are material damage parameters, which are currently assumed to be independent of strain-rate. The damage function is formulated to account for the overall nonlinear elastic response of a lamina including the initial ‘hardening’ and the subsequent softening beyond the ultimate strengths. In the damage model (material 162), the effect of strain-rate on the nonlinear stress- strain response of a composite layer is modeled by the strain-rate dependent functions for the elastic moduli {𝐸𝑅𝑇 } as {𝐸𝑅𝑇 } = {𝐸0 } (1 + {𝐶rate} ln ̇} {𝜀̅ ) 𝜀̇0 {𝐸𝑅𝑇 } = ⎧ 𝐸𝑎 ⎫ }} {{ 𝐸𝑏 }} {{ 𝐸𝑐 ⎬ ⎨ 𝐺𝑎𝑏 }} {{ 𝐺𝑏𝑐 }} {{ 𝐺𝑐𝑎⎭ ⎩ {𝜀̅ ̇} = ⎧ ∣𝜀̇𝑎∣ ⎫ } { } { ∣𝜀̇𝑏∣ } { } { ∣𝜀̇𝑐∣ ⎬ ⎨ ∣𝜀̇𝑎𝑏∣ } { } { ∣𝜀̇𝑏𝑐∣ } { } { ∣𝜀̇𝑐𝑎∣⎭ ⎩ {𝐶rate} = ⎧𝐶rate2 ⎫ } { } { 𝐶rate2 } { } { 𝐶rate4 ⎬ ⎨ 𝐶rate3 } { } { 𝐶rate3 } { } { 𝐶rate3⎭ ⎩ where {𝐶rate} are the strain-rate constants. {𝐸0 } are the modulus values of {𝐸𝑅𝑇 } at the reference strain-rate 𝜀̇0. Element Erosion: A failed element is eroded in any of three different ways: 1. 2. 3. If fiber tensile failure in a unidirectional layer is predicted in the element and the axial tensile strain is greater than E_LIMT. For a fabric layer, both in-plane directions are failed and exceed E_LIMT. If compressive relative volume in a failed element is smaller than ECRSH. If tensile relative volume in a failed element is greater than EEXPN. Damage History Parameters: Information about the damage history variables for the associated failure modes can be plotted in LS-PrePost. These additional history variables are tabulated below: History Variable Description Value LS-PrePost History Variable 1. efa(I) Fiber mode in a 2. efb(I) Fiber mode in b 0-elastic 3. efp(I) Fiber crush mode 4. em(I) 5. ed(I) Perpendicular matrix mode Parallel matrix/ delamination mode 6. delm(I) delamination mode ≥1-failed 7 8 9 10 11 12 *MAT_MODIFIED_CRUSHABLE_FOAM This is Material Type 163 which is dedicated to modeling crushable foam with optional damping, tension cutoff, and strain rate effects. Unloading is fully elastic. Tension is treated as elastic-perfectly-plastic at the tension cut-off value. Card 1 1 Variable MID 2 RO Type A8 F 3 E F 4 PR F 5 TID 6 7 8 TSC DAMP NCYCLE F F F F Default none none none none none 0.0 0.10 12. Card 2 1 2 3 4 5 6 7 8 Variable SRCLMT SFLAG Type F Default 1.E+20 I 0 VARIABLE DESCRIPTION MID RO E PR TID TSC Material identification. A unique number or label not exceeding 8 characters must be specified. Mass density Young’s modulus Poisson’s ratio Table ID defining yield stress versus volumetric strain, γ, at different strain rates. Tensile stress cutoff. A nonzero, positive value is strongly recommended for realistic behavior. DAMP Rate sensitivity via damping coefficient (.05 < recommended value<.50). > > 1-V Figure M163-1. Rate effects are defined by a family of curves giving yield stress versus volumetric strain where V is the relative volume. VARIABLE DESCRIPTION NCYCLE Number of cycles to determine the average volumetric strain rate. SRCLMT Strain rate change limit. SFLAG The strain rate in the table may be the true strain rate (SFLAG = 0) or the engineering strain rate (SFLAG = 1). Remarks: The volumetric strain is defined in terms of the relative volume, V, as: 𝛾 = 1 − V The relative volume is defined as the ratio of the current to the initial volume. In place of the effective plastic strain in the D3PLOT database, the integrated volumetric strain is output. This material is an extension of material 63, *MAT_CRUSHABLE_FOAM. It allows the yield stress to be a function of both volumetric strain rate and volumetric strain. Rate effects are accounted for by defining a table of curves using *DEFINE_TABLE. Each curve defines the yield stress versus volumetric strain for a different strain rate. The yield stress is obtained by interpolating between the two curves that bound the strain rate. To prevent high frequency oscillations in the strain rate from causing similar high frequency oscillations in the yield stress, a modified volumetric strain rate is used when interpolating to obtain the yield stress. The modified strain rate is obtained as follows. If NYCLE is > 1, then the modified strain rate is obtained by a time average of the actual strain rate over NCYCLE solution cycles. For SRCLMT > 0, the modified strain rate is capped so that during each cycle, the modified strain rate is not permitted to change more than SRCLMT multiplied by the solution time step. *MAT_BRAIN_LINEAR_VISCOELASTIC This is Material Type 164. This material is a Kelvin-Maxwell model for modeling brain tissue, which is valid for solid elements only. See Remarks below. Card 1 1 Variable MID 2 RO 3 BULK Type A8 F F 4 G0 F 5 GI F 6 DC F 7 FO F 8 SO F Default none none none none none 0.0 0.0 0.0 VARIABLE MID DESCRIPTION Material identification. A unique number or label not exceeding 8 characters must be specified. RO Mass density BULK Bulk modulus (elastic) G0 GI DC FO Short-time shear modulus, G0 Long-time (infinite) shear modulus, G∞ Maxwell decay constant, β[FO = 0.0] or Kelvin relaxation constant, τ [FO = 1.0] Formulation option: EQ.0.0: Maxwell, EQ.1.0: Kelvin. VARIABLE SO DESCRIPTION Strain (logarithmic) output option to control what is written as component 7 to the d3plot database. (LS-PrePost always blindly labels this component as effective plastic strain.) The maximum values are updated for each element each time step: EQ.0.0: maximum principal strain that occurs during the calculation, EQ.1.0: maximum magnitude of the principal strain values that occurs during the calculation, EQ.2.0: maximum effective strain that occurs during the calculation. Remarks: The shear relaxation behavior is described for the Maxwell model by: A Jaumann rate formulation is used 𝐺(𝑡) = 𝐺 + (𝐺0 − 𝐺∞)𝑒−𝛽𝑡 𝛻 𝑖𝑗 = 2 ∫ 𝐺(𝑡 − 𝜏)𝐷𝑖𝑗 ′ (𝜏)𝑑𝑡 ∇ 𝑖𝑗, and the strain rate Dij . where the prime denotes the deviatoric part of the stress rate, 𝜎 For the Kelvin model the stress evolution equation is defined as: 𝑠 ̇𝑖𝑗 + 𝑠𝑖𝑗 = (1 + 𝛿𝑖𝑗)𝐺0𝑒 ̇𝑖𝑗 + (1 + 𝛿𝑖𝑗) 𝐺∞ 𝑒 ̇𝑖𝑗 The strain data as written to the d3plot database may be used to predict damage, see [Bandak 1991]. *MAT_PLASTIC_NONLINEAR_KINEMATIC This is Material Type 165. This relatively simple model, based on a material model by Lemaitre and Chaboche [1990], is suited to model nonlinear kinematic hardening plasticity. The model accounts for the nonlinear Bauschinger effect, cyclic hardening, and ratcheting. Huang [2006] programmed this model and provided it as a user subroutine. It is a very cost effective model and is available shell and solid elements. Card 1 1 Variable MID 2 RO Type A8 F 3 E F 4 PR F 5 SIGY F 6 H F 7 C F 8 GAMMA F Default none none none none none 0.0 0.0 0.0 2 3 4 5 6 7 8 Card 2 Variable 1 FS Type F Default 1.E+16 VARIABLE DESCRIPTION MID RO E PR Material identification. A unique number or label not exceeding 8 characters must be specified. Mass density. Young’s modulus. Poisson’s ratio. SIGY Initial yield stress, 𝜎𝑦0. H C Isotropic plastic hardening modulus Kinematic hardening modulus VARIABLE DESCRIPTION GAMMA Kinematic hardening parameter, 𝛾. FS Failure strain for eroding elements. Remarks: If the isotropic hardening modulus, H, is nonzero, the size of the surface increases as function of the equivalent plastic strain,𝜀𝑝: 𝜎𝑦 = 𝜎𝑦0 + 𝐻𝜀𝑝 The rate of evolution of the kinematic component is a function of the plastic strain rate: 𝛼̇ = [𝐶𝑛 − 𝛾𝛼]𝜀̇𝑝 where, n, is the flow direction. The term, 𝛾𝛼𝜀̇𝑝, introduces the nonlinearity into the evolution law, which becomes linear if the parameter, 𝛾, is set to zero. *MAT_PLASTIC_NONLINEAR_KINEMATIC_B This is Material Type 165B. This material model is implemented to model the cyclic fatigue behavior. This model applies to both shell and solid elements. Card 1 1 Variable MID 2 RO Type A8 F 3 E F 4 PR F 5 RE F 6 B F 7 Q F 8 C1 F Default none none none none none none none none Card 2 1 2 3 4 5 6 7 8 Variable GAMMA1 C2 GAMMA2 C3 GAMMA3 Type F F F F F Default none none none none none VARIABLE MID DESCRIPTION Material identification. A unique number or label not exceeding 8 characters must be specified. RO E PR RE B Q Mass density. Young’s Modulus Poisson’s ratio Yield stress, see Remarks. Material parameter, see Remarks. Material parameter, see Remarks. VARIABLE DESCRIPTION Material parameters, see Remarks. C1, GAMMA1, C2, GAMMA2, C3, GAMMA3 A model of elastoplatic cyclic hardening: This material model is based on a 2013 paper by S. Plessis which modeled a double- notched specimen with Herbland (2009) material model. The elstoplastic stress tensor is given by: 𝜎 = 𝜎𝑀 − 𝐿: ε𝑝 where, 𝜎𝑀 is elastic stress, ε𝑝 is the plastic strain tensor. In a one-dimensional problem, the above equation becomes: where, 𝐿′ is a parameter identified with FEM on a monotonic loading. 𝜎 = 𝜎𝑀 − 𝐿′ε𝑝 In the elasticity domain: 𝑓 = 𝐽2(𝜎 − 𝑋𝑇) − 𝑅𝑒 − 𝑅 ≤ 0 where 𝐽2 is the second stress invariant, 𝜎 is the stress tension, 𝑅 is the isotropic hardening variable, 𝑅𝑒 (variable RE) is the yield stress. Evolution law of the isotropic hardening variable R: 𝑅̇ = 𝑏 𝑋(𝑄 − 𝑅)𝑝̇ where 𝑏 (variable B) and 𝑄 (variable Q) are two material parameters, 𝑝̇ is the plastic strain rate defined by: 𝑝̇ = √ 𝜖 ̇𝑝: 𝜖 ̇𝑝 with 𝜖 ̇𝑝 the plastic strain tensor. Evolution law of the variable of kinematic hardening: with, 𝑋𝑇̇ = ∑ 𝑋𝚤̇ 𝑋𝚤̇ = 𝐶𝑖𝜖 ̇𝑝 − 𝛾𝑖𝑋𝑖𝑝̇ where 𝑋𝑇̇ is the kinematic hardening tensor, and is the sum of three tensors 𝑋𝚤̇ (𝑖 = 1~3), each dependent on the one set of material coefficients 𝐶𝑖 (variables C1, C2, C3) and 𝛾𝑖(variables GAMMA1, GAMMA2, GAMMA3). Revision information: This material model is available starting in Revision 102594. *MAT_MOMENT_CURVATURE_BEAM This is Material Type 166. This material is for performing nonlinear elastic or multi- linear plastic analysis of Belytschko-Schwer beams with user-defined axial force-strain, moment curvature and torque-twist rate curves. If strain, curvature or twist rate is located outside the curves, use extrapolation to determine the corresponding rigidity. For multi-linear plastic analysis, the user-defined curves are used as yield surfaces. Card 1 1 Variable MID 2 RO Type A8 F 3 E F 4 5 6 7 8 ELAF EPFLG CTA CTB CTT F F F F F Default none none none none 0.0 0.0 0.0 0.0 Card 2 Variable 1 N1 Type F 2 N2 F Default none none 3 N3 F 0.0 / none 4 N4 F 5 N5 F 6 N6 F 7 N7 F 8 N8 F 0.0 0.0 0.0 0.0 0.0 Card 3 1 2 3 4 5 6 7 8 Variable LCMS1 LCMS2 LCMS3 LCMS4 LCMS5 LCMS6 LCMS7 LCMS8 Type F F F F F F F F Default none none 0.0 / none 0.0 0.0 0.0 0.0 0.0 Card 4 1 2 3 4 5 6 7 8 Variable LCMT1 LCMT2 LCMT3 LCMT4 LCMT5 LCMT6 LCMT7 LCMT8 Type F F F F F F F F Default none none 0.0 / none 0.0 0.0 0.0 0.0 0.0 Card 5 1 2 3 4 5 6 7 8 Variable LCT1 LCT2 LCT3 LCT4 LCT5 LCT6 LCT7 LCT8 Type F F F F F F F F Default none none 0.0 / none 0.0 0.0 0.0 0.0 0.0 Multilinear Plastic Analysis Card. Additional card for EPFLG = 1. Card 6 1 2 3 4 5 6 7 8 Variable CFA CFB CFT HRULE REPS RBETA RCAPAY RCAPAZ Type F F F F F F F F Default 1.0 1.0 1.0 0.0 1.0E+20 1.0E+20 1.0E+20 1.0E+20 VARIABLE DESCRIPTION MID RO E Material identification. A unique number or label not exceeding 8 characters must be specified. Mass density Young’s modulus. This variable controls the time step size and must be chosen carefully. Increasing the value of E will decrease the time step size. VARIABLE DESCRIPTION ELAF Load curve ID for the axial force-strain curve EPFLG Function flag EQ.0.0: nonlinear elastic analysis EQ.1.0: multi-linear plastic analysis CTA, CTB, CTT Type of axial force-strain, moment-curvature, and torque-twist rate curves EQ.0.0: curve is symmetric EQ.1.0: curve is asymmetric For symmetric curves, all data point must be in the first quadrant and at least three data points need to be given, starting from the origin, ensued by the yield point. For asymmetric curves, at least five data points are needed and exactly one point must be at the origin. The two points on both sides of the origin record the positive and negative yield points. The last data point(s) has no physical meaning: it serves only as a control point for inter or extrapolation. The curves are input by the user and treated in LS-DYNA as a linearly piecewise function. The curves must be monotonically increasing, while the slopes must be monotonically decreasing Axial forces at which moment-curvature curves are given. The axial forces must be ordered monotonically increasing. At least two axial forces must be defined if the curves are symmetric. At least three axial forces must be defined if the curves are asymmetric. Load curve IDs for the moment-curvature curves about axis S under corresponding axial forces. Load curve IDs for the moment-curvature curves about axis T under corresponding axial forces. Load curve corresponding axial forces. IDs for the torque-twist rate curves under For multi-linear plastic analysis only. Ratio of axial, bending and torsional elastic rigidities to their initial values, no less than 1.0 in value. N1 - N8 LCMS1 - LCMS8 LCMT1 - LCMT8 LCT1 - LCT8 CFA, CFB, CFT *MAT_MOMENT_CURVATURE_BEAM DESCRIPTION HRULE Hardening rule, for multi-linear plastic analysis only. EQ.0.0: isotropic hardening GT.0.0.AND.LT.1.0: mixed hardening EQ.1.0: kinematic hardening REPS Rupture effective plastic axial strain RBETA Rupture effective plastic twist rate RCAPAY Rupture effective plastic curvature about axis S RCAPAZ Rupture effective plastic curvature about axis T *MAT_167 This is Material Type 167. This is a constitute model for finite plastic deformities in which the material’s strength is defined by McCormick’s constitutive relation for materials exhibiting negative steady-state Strain Rate Sensitivity (SRS). McCormick [1988] and Zhang, McCormick and Estrin [2001]. Card 1 1 Variable MID 2 RO Type A8 F Card 2 Variable 1 Q1 Type F Card 3 Variable Type 1 S F 2 C1 F 2 H F 3 E F 3 Q2 F 3 4 PR F 4 C2 F 4 5 6 7 8 SIGY F 5 6 7 8 5 6 7 8 OMEGA TD ALPHA EPS0 F F F F VARIABLE DESCRIPTION MID RO E PR Material identification. A unique number or label not exceeding 8 characters must be specified. Mass density. Young’s modulus. Poisson’s ratio. SIGY Initial yield stress Q1 C1 Isotropic hardening parameter, 𝑄1 Isotropic hardening parameter, 𝐶1 VARIABLE Q2 C2 S H DESCRIPTION Isotropic hardening parameter, 𝑄2 Isotropic hardening parameter, 𝐶2 Dynamic strain aging parameter, 𝑆 Dynamic strain aging parameter, 𝐻 OMEGA Dynamic strain aging parameter, Ω TD Dynamic strain aging parameter, 𝑡𝑑 ALPHA Dynamic strain aging parameter, 𝛼 EPS0 Reference strain rate, 𝜀̇0 Remarks: The uniaxial stress-strain curve is given in the following form: 𝜎(𝜀𝑝, 𝜀̇𝑝) = 𝜎𝑌(𝑡𝑎) + 𝑅(𝜀𝑝) + 𝜎𝑣(𝜀̇𝑝) Viscous stress 𝜎𝑣 is given by 𝜎𝑣(𝜀̇𝑝) = S × ln (1 + 𝜀̇𝑝 𝜀̇𝑜 ) where 𝑆 represents the instantaneous strain rate sensitivity and 𝜀̇𝑜 is a reference strain rate. In the McCormick model the yield strength including the contribution from dynamic strain again (DSA) is defined as 𝜎𝑌(𝑡𝑎) = 𝜎𝑜 + S × H × [1 − exp {− ( ) 𝑡𝑎 𝑡𝑑 }] where 𝜎𝑜 is the yield strength for vanishing average waiting time 𝑡𝑎, and 𝐻, 𝛼, and 𝑡𝑑 are material constants linked to dynamic strain aging. The average waiting time is defined by the evolution equation 𝑡 ̇𝑎 = 1 − 𝑡𝑎 𝑡𝑎,𝑠𝑠 where the quasi-steady state waiting time 𝑡𝑎,𝑠𝑠 is given as 𝑡𝑎,𝑠𝑠 = 𝜀̇𝑝. The strain hardening function 𝑅 is defined by the extended Voce Law 𝑅(𝜀𝑝) = 𝑄1[1 − exp(−𝐶1𝜀𝑝)] + 𝑄2[1 − exp(−𝐶2𝜀𝑝)]. *MAT_POLYMER This is material type 168. This model is implemented for brick elements. Card 1 1 Variable MID Type A8 Card 2 1 Variable TEMP Type F 2 RO F 2 K F 3 E F 3 CR F 4 5 6 PR GAMMA0 DG F 6 F 4 N F F 5 C F VARIABLE DESCRIPTION 7 SC F 7 8 ST F 8 MID RO E PR Material identification. A unique number or label not exceeding 8 characters must be specified. Mass Density. Young’s modulus, 𝐸. Poisson’s ratio, 𝜈. GAMMA0 Pre-exponential factor, 𝛾̇0𝐴. DG SC ST Energy barrier to flow, Δ𝐺. Shear resistance in compression, 𝑆𝑐. Shear resistance in tension, 𝑆𝑡. TEMP Absolute temperature, 𝜃. K CR N C Boltzmann constant, 𝑘. Product, 𝐶𝑟 = 𝑛𝑘𝜃. Number of ‘rigid links’ between entanglements, 𝑁. Relaxation factor, 𝐶. *MAT_168 The polymer is assumed to have two basic resistances to deformation: Elastic stiffness (Hooke's law) Plastic flow (Argon's model) A B Network stiffness (Arruda- Boyce model) Total A (Inter-molecular) B (Network) True strain Figure M168-1. Stress decomposition in inter-molecular and network contributions. 1. An inter-molecular barrier to deformation related to relative movement between molecules. 2. An evolving anisotropic resistance related to straightening of the molecule chains. The model which is implemented and presented in this paper is mainly based on the framework suggested by Boyce et al. [2000]. Going back to the original work by Haward and Thackray [1968], they considered the uniaxial case only. The extension to a full 3D formulation was proposed by Boyce et al. [1988]. Moreover, Boyce and co- workers have during a period of 20 years changed or further developed the parts of the original model. Haward and Thackray [1968] used an Eyring model to represent the dashpot in Fig. M168-1, while Boyce et al. [2000] employed the double-kink model of Argon [1973] instead. Part B of the model, describing the resistance associated with straightening of the molecules, contained originally a one-dimensional Langevin spring [Haward and Thackray, 1968], which was generalized to 3D with the eight-chain model by Arruda and Boyce [1993]. The main structure of the model presented by Boyce et al. [2000] is kept for this model. Recognizing the large elastic deformations occurring for polymers, a formulation based on a Neo-Hookean material is here selected for describing the spring in resistance A in Figure M168-1. Referring to Figure M168-1, it is assumed that the deformation gradient tensor is the same for the two resistances (Part A and B) while the Cauchy stress tensor for the system is assumed to be the sum of the Cauchy stress tensors for the two parts 𝐅 = 𝐅𝐴 = 𝐅𝐵 σ = σ𝐴 + σ𝐵. Part A: Inter-molecular resistance: 𝑝 , where it is The deformation is decomposed into elastic and plastic parts, 𝐅𝐴 = 𝐅𝐴 𝑝 is invariant to rigid assumed that the intermediate configuration Ω̅̅̅̅̅̅𝐴 defined by 𝐅𝐴 body rotations of the current configuration. The velocity gradient in the current configuration Ω is defined by 𝑒 ⋅ 𝐅𝐴 Owing to the decomposition, 𝐅𝐴 = 𝐅𝐴 and spin tensors are defined by 𝐋𝐴 = 𝐅̇𝐴 ⋅ 𝐅𝐴 𝑒 ⋅ 𝐅𝐴 𝑝 𝑒 + 𝐋𝐴 −1 = 𝐋𝐴 𝑝 , the elastic and plastic rate-of-deformation 𝑒 + 𝐖𝐴 𝑝 + 𝐖𝐴 𝑒 = 𝐅̇ 𝑝 = 𝐅𝐴 𝑒 ⋅ (𝐅𝐴 𝑒 ⋅ 𝐅̇ 𝑒 )−1 𝑝 ⋅ (𝐅𝐴 𝑝 )−1 ⋅ (𝐅𝐴 𝑒 )−1 = 𝐅𝐴 𝑒 ⋅ 𝐋̅ 𝑝 ⋅ (𝐅𝐴 𝑒 )−1 𝑒 = 𝐃𝐴 𝐋𝐴 𝑝 = 𝐃𝐴 𝐋𝐴 𝑝 ⋅ (𝐅𝐴 𝑝 = 𝐅̇ 𝑝 )−1. The Neo-Hookean material represents an extension of Hooke's where 𝐋̅ law to large elastic deformations and may be chosen for the elastic part of the deformation when the elastic behavior is assumed to be isotropic. τ𝐴 = 𝜆0ln𝐽𝐴 𝑒 𝐈 + 𝜇0(𝐁𝐴 𝑒 − 𝐈) 𝑒 = 𝐽𝐴 is the where τ𝐴 = 𝐽𝐴σ𝐴 is the Kirchhoff stress tensor of Part A and 𝐽𝐴 Jacobian determinant. The elastic left Cauchy-Green deformation tensor is given by 𝑒 = 𝐅𝐴 𝐁𝐴 𝑒 = √det𝐁𝐴 𝑒 ⋅ 𝐅𝐴 𝑒 𝑇. The flow rule is defined by where 𝑝 = 𝛾̇𝐴 𝐋𝐴 𝑝 𝐍𝐴 𝐍𝐴 = √2 𝜏𝐴 dev, τ𝐴 𝜏𝐴 = √ dev) tr(τ𝐴 𝑑𝑒𝑣 is the stress deviator. The rate of flow is taken to be a thermally activated and τ𝐴 process 𝑝 = 𝛾̇0𝐴exp [− 𝛾̇𝐴 Δ𝐺(1 − 𝜏𝐴/𝑠) 𝑘𝜃 ] where 𝛾̇0𝐴 is a pre-exponential factor, Δ𝐺 is the energy barrier to flow, 𝑠 is the shear resistance, 𝑘 is the Boltzmann constant and 𝜃 is the absolute temperature. The shear resistance 𝑠 is assumed to depend on the stress triaxiality 𝜎 ∗, 𝑠 = 𝑠(𝜎 ∗), 𝜎 ∗ = tr σ𝐴 3√3𝜏𝐴 The exact dependence is given by a user-defined load curve, which is linear between the shear resistances in compression and tension. These resistances are denoted sc and st, respectively. Part B: Network resistance: The network resistance is assumed to be nonlinear elastic with deformation gradient 𝑁, i.e. any viscoplastic deformation of the network is neglected. The stress- 𝐅𝐵 = 𝐅𝐵 stretch relation is defined by τ𝐵 = 𝑛𝑘𝜃 √𝑁 𝜆̅̅̅̅𝑁 ℒ −1 ⎜⎛ 𝜆̅̅̅̅𝑁 √𝑁⎠ ⎝ ⎟⎞ (𝐁̅̅̅̅ 𝑁 − 𝜆̅̅̅̅ 2 𝐈) where τ𝐵 = 𝐽𝐵σ𝐵 is the Kirchhoff stress for Part B, 𝑛 is the chain density and 𝑁 the number of ‘rigid links’ between entanglements. In accordance with Boyce et. al [2000], the product, 𝑛𝑘𝜃 is denoted 𝐶𝑅 herein. Moreover, ℒ −1 is the inverse Langevin function, ℒ(𝛽) = coth𝛽 − 1 𝛽⁄ , and further 𝐁̅̅̅̅ 𝑁 = 𝐅̅̅̅̅ 𝑁 ⋅ 𝐅̅̅̅̅ 𝑁 𝑇 , 𝐅̅̅̅̅ 𝑁 = 𝐽𝐵 −1/3 𝐅𝐵 𝑁, 𝐽𝐵 = det𝐅𝐵 𝑁, 𝜆̅̅̅̅𝑁 = [ tr 𝐁̅̅̅̅ 𝑁] The flow rule defining the rate of molecular relaxation reads 𝐹 = 𝛾̇𝐵 𝐋𝐵 𝐹𝐍𝐵 where 𝐍𝐵 = √2 𝜏𝐵 dev, τ𝐵 𝜏𝐵 = √ dev: τ𝐵 τ𝐵 dev The rate of relaxation is taken equal to where 𝐹 = 𝐶 ( 𝛾̇𝐵 𝜆̅̅̅̅𝐹 − 1 ) 𝜏𝐵 𝜆̅̅̅̅𝐹 = [ tr(𝐅𝐵 𝐹} 𝐹{𝐅𝐵 )] The model has been implemented into LS-DYNA using a semi-implicit stress-update scheme [Moran et. al 1990], and is available for the explicit solver only. *MAT_169 This is Material Type 169. This material model was written for adhesive bonding in aluminum structures. The plasticity model is not volume-conserving, and hence avoids the spuriously high tensile stresses that can develop if adhesive is modeled using traditional elasto-plastic material models. It is available only for solid elements of formulations 1, 2 and 15. The smallest dimension of the element is assumed to be the through-thickness dimension of the bond, unless THKDIR = 1. Card 1 1 Variable MID 2 RO Type A8 F 3 E F 4 5 6 7 8 PR TENMAX GCTEN SHRMAX GCSHR F F F F F Default none none none none 1020 1020 1020 1020 Card 2 1 2 3 4 5 6 7 8 Variable PWRT PWRS SHRP SHT_SL EDOT0 EDOT2 THKDIR EXTRA Type F F F F F F F F Default 2.0 2.0 0.0 0.0 1.0 0.0 0.0 0.0 Additional card for Extra = 1 or 3. Card 3 1 2 3 4 5 6 7 8 Variable TMAXE GCTE SMAXE GCSE PWRTE PWRSE Type F F F F F F Default 1020 1020 1020 1020 2.0 2.0 *MAT_ARUP_ADHESIVE Card 4 1 2 3 4 5 6 7 8 Variable FACET FACCT FACES FACCS SOFTT SOFTS Type F F F F F F Default 1.0 1.0 1.0 1.0 1.0 1.0 Dynamic Strain Rate Card. Additional card for EDOT2 ≠ 0. Card 5 1 2 3 4 5 6 7 8 Variable SDFAC SGFAC SDEFAC SGEFAC Type F F F F Default 1.0 1.0 1.0 1.0 Bond Thickness Card. Additional card for Extra = 2 or 3. Card 6 1 2 3 4 5 6 7 8 Variable BTHK OUTFAIL FSIP Type F F F Default 0.0 0.0 0.0 VARIABLE DESCRIPTION MID RO E PR Material identification. A unique number or label not exceeding 8 characters must be specified. Mass density. Young’s modulus. Poisson’s ratio. VARIABLE DESCRIPTION TENMAX Maximum through-thickness tensile stress GT.0.0: constant value LT.0.0: |TENMAX| is ID of a *DEFINE_FUNCTION GCTEN Energy per unit area to fail the bond in tension GT.0.0: constant value LT.0.0: |GCTEN| is ID of a *DEFINE_FUNCTION SHRMAX Maximum through-thickness shear stress GT.0.0: constant value LT.0.0: |SHRMAX| is ID of a *DEFINE_FUNCTION GCSHR Energy per unit area to fail the bond in shear GT.0.0: constant value LT.0.0: |GCSHR| is ID of a *DEFINE_FUNCTION Power law term for tension Power law term for shear Shear plateau ratio (Optional) GT.0.0: constant value LT.0.0: |SHRP| Remarks) is ID of a *DEFINE_FUNCTION of yield surface at zero tension EDOT0 Strain rate at which the “static” properties apply EDOT2 Strain rate at which the “dynamic” properties apply (Card 5) THKDIR Through-thickness direction flag EQ.0.0: smallest element dimension (default) EQ.1.0: direction from nodes 1-2-3-4 to nodes 5-6-7-8 *MAT_ARUP_ADHESIVE DESCRIPTION EXTRA Flag to input further data: EQ.1.0: interfacial failure properties (cards 3 and 4) EQ.2.0: bond thickness and more (card 6) EQ.3.0: both of the above TMAXE Maximum tensile force per unit length on edges of joint GCTE Energy per unit length to fail the edge of the bond in tension SMAXE Maximum shear force per unit length on edges of joint GCSE Energy per unit length to fail the edge of the bond in shear PWRTE Power law term for tension PWRSE Power law term for shear FACET Stiffness scaling factor for edge elements – tension FACCT Stiffness scaling factor for interior elements – tension FACES Stiffness scaling factor for edge elements – shear FACCS Stiffness scaling factor for interior elements – shear SOFTT SOFTS Factor by which the tensile strength is reduced when a neighbor fails Factor by which the shear strength is reduced when a neighbor fails SDFAC Factor on TENMAX and SHRMAX at strain rate EDOT2 GT.0.0: constant value LT.0.0: |SDFAC| Remarks) is ID of a *DEFINE_FUNCTION is ID of a *DEFINE_FUNCTION (see SDEFAC Factor on TMAXE and SMAXE at strain rate EDOT2 VARIABLE DESCRIPTION SGEFAC Factor on GCTE and GCSE at strain rate EDOT2 BTHK Bond thickness (overrides thickness from element dimensions) LT.0.0: |BTHK| is bond thickness, but critical time step remains unaffected. Helps to avoid very small time steps, but it can affect stability. OUTFAIL Flag for additional output to messag file: Information about damage initiation time, failure function terms and forces. EQ.0.0: off EQ.1.0: on FSIP Effective in-plane strain at failure. Remarks: The through-thickness direction is identified from the smallest dimension of each element by default (THKDIR = 0.0). It is expected that this dimension will be smaller than in-plane dimensions (typically 1-2mm compared with 5-10mm). If this is not the through-thickness direction via element numbering case, one can set (THKDIR = 1.0). Then the thickness direction is expected to point from lower face (nodes 1-2-3-4) to upper face (nodes 5-6-7-8). For wedge elements these faces are the two triangular faces (nodes 1-2-5) and (nodes 3-4-6). the The bond thickness is assumed to be the element size in the thickness direction. This may be overridden using BTHK. In this case the behavior becomes independent of the element thickness. The elastic stiffness is affected by BTHK, so it is necessary to set the characteristic element length to a smaller value new = √BTHK × 𝑙𝑒 𝑙𝑒 old. This again affects the critical time step of the element, i.e. a small BTHK can decrease the element time step significantly. In-plane stresses are set to zero: it is assumed that the stiffness and strength of the substrate is large compared with that of the adhesive, given the relative thicknesses. If the substrate is modeled with shell elements, it is expected that these will lie at the mid-surface of the substrate geometry. Therefore the solid elements representing the adhesive will be thicker than the actual bond. If the elastic compliance of the bond is significant, this can be corrected by increasing the elastic stiffness property E. SHT_SL > 0 SHT_SL = 0 shear stress SHRMAX direct stress TENMAX Figure M169-1. Figure illustrating the yield surface. The yield and failure surfaces are treated as a power-law combination of direct tension and shear across the bond: ( 𝜎max PWRT + ( ) 𝜏max − SHT_ SL × 𝜎 PWRS = 1.0 ) At yield SHT_SL is the slope of the yield surface at 𝜎 = 0. See Figure M169-1 The stress-displacement curves for tension and shear are shown in Figure M169-2. In both cases, GC is the area under the curve. The displacement to failure in tension is given by subject to a lower limit 𝑑ft = 2 ( GCTEN TENMAX ) , 𝑑ft, min = ( 2𝐿0 𝐸′ ) TENMAX where 𝐿0 is the initial element thickness (or BTHK if used) and 𝐸′ = 𝐸(1 − 𝜈) (1 − 2𝜈)(1 + 𝜈) . If GCTEN is input such that 𝑑ft < 𝑑ft, min, LS-DYNA will automatically increase GCTEN to make 𝑑ft = 𝑑ft, min. Therefore, GCTEN has a minimum value of dp = SHRP × dfs TENAMX Area = GCten Failure (dft) SHRMAX Area = GCshr Failure (dfs) Displacement (Tension) Displacement (Shear) Figure M169-2. Stress-Displacement Curves for Tension and Shear. σMAX/TENMAX SDFAC 1.0 Log(plastic strain rate) Log(EDOT0) Log(EDOT2) Figure M169-3. Figure illustrating rate effects. Similarly, the minimum value for GCSHR is GCTEN ≥ 𝐿0 𝐸′ (TENMAX)2 GCSHR ≥ 𝐿0 (SHRMAX)2 where 𝐺 is the elastic shear modulus. Because of the algorithm used, yielding in tension across the bond does not require strains in the plane of the bond – unlike the plasticity models, plastic flow is not treated as volume-conserving. The Plastic Strain output variable has a special meaning: 0 < PS < 1: PS is the maximum value of the yield function experienced since time zero 1 < PS < 2: the element has yielded and the strength is reducing towards failure – yields at PS = 1, fails at PS = 2. The damage cause by cohesive deformation (0 at first yield to 1 at failure) and by interfacial deformation are stored in the first two extra history variables. These can be plotted if NEIPH on *DATABASE_EXTENT_BINARY is 2 or more. By this means, the reasons for failure may be assessed. When the plastic strain rate rises above EDOT0, rate effects are assumed to scale with the logarithm of the lastic strain rate, as in the example shown in Figure M169-3 for cohesive tensile strength with dynamic factor SDFAC. The same form of relationship is applied for the other dynamic factors. If EDOT0 is zero or blank, no rate effects are applied. Rate effects are applied using the viscoplastic method. Interfacial failure is assumed to arise from stress concentrations at the edges of the bond – typically the strength of the bond becomes almost independent of bond length. This type of failure is usually more brittle than cohesive failure. To simulate this, LS-DYNA identifies the free edges of the bond (made up of element faces that are not shared by other elements of material type *MAT_ARUP_ADHESIVE, excluding the faces that bond to the substrate). Only these elements can fail initially. The neighbors of failed elements can then develop free edges and fail in turn. In real adhesive bonds, the stresses at the edges can be concentrated over very small areas; in typical finite element models the elements are much too large to capture this. Therefore the concentration of loads onto the edges of the bond is accomplished artificially, by stiffening elements containing free edges (e.g. FACET, FACES > 1) and reducing the stiffness of interior elements (e.g. FACCT, FACCS < 1). Interior elements are allowed to yield at reduced loads (equivalent to TMAXE × FACET/FACCT and SMAXE × FACES/FACCS) to prevent excessive stresses developing before the edge elements have failed - but cannot be damaged until they become edge elements after the failure of their neighbors. Parameters TENMAX, GCTEN, SHRMAX, GCSHR, SHRP, SDFAC, and SGFAC can be defined as negative values. to *DEFINE_FUNCTION ID’s. The arguments of those functions include several properties of both connection partners if corresponding solid elements are in a tied contact with shell elements. the absolute values refer that case, In These functions depend on: (t1, t2) = thicknesses of both bond partners (sy1, sy2) = initial yield stresses at plastic strain of 0.002 (sm1, sm2) = maximum engineering yield stresses (necking points) r = strain rate a = element area For TENMAX = -100 such a function could look like: *DEFINE_FUNCTION 100 func(t1,t2,sy1,sy2,sm1,sm2,r,a)=0.5*(sy1+sy2) Since material parameters have to be identified from both bond partners during initialization, this feature is only available for a subset of material models at the moment, namely no. 24, 120, 123, and 124. *MAT_RESULTANT_ANISOTROPIC This is Material Type 170. This model is available the Belytschko-Tsay and the C0 triangular shell elements and is based on a resultant stress formulation. In-plane behavior is treated separately from bending in order to model perforated materials such as television shadow masks. The plastic behavior of each resultant is specified with a load curve and is completely uncoupled from the other resultants. If other shell formulations are specified, the formulation will be automatically switched to Belytschko-Tsay. As implemented, this material model cannot be used with user defined integration rules. NOTE: This material does not support specification of a ma- terial angle, 𝛽𝑖, for each through-thickness integra- tion point of a shell. Card 1 1 Variable MID Type A8 Card 2 1 2 RO F 2 3 4 5 6 7 8 3 4 5 6 7 8 Variable E11P E22P V12P V21P G12P G23P G31P Type F Card 3 1 F 2 F 3 F 4 F 5 F 6 F 7 8 Variable E11B E22B V12B V21B G12B AOPT Type F F F F F Card 4 1 2 3 4 5 6 7 8 Variable LN11 LN22 LN12 LQ1 LQ2 LM11 LM22 LM12 Type F Card 5 1 Variable Type Card 6 Variable 1 V1 Type F F 2 2 V2 F F 3 3 V3 F F F F 4 A1 F 4 D1 F 5 A2 F 5 D2 F 6 A3 F 6 D3 F F 7 F 8 7 8 BETA F VARIABLE DESCRIPTION MID RO E11P E22P V12P V11P G12P G23P G31P E11B Material identification. A unique number or label not exceeding 8 characters must be specified. Mass density. 𝐸11𝑝, for in plane behavior. 𝐸22𝑝, for in plane behavior. 𝜈12𝑝, for in plane behavior. 𝜈11𝑝, for in plane behavior. 𝐺12𝑝, for in plane behavior. 𝐺23𝑝, for in plane behavior. 𝐺31𝑝, for in plane behavior. 𝐸11𝑏, for bending behavior. VARIABLE DESCRIPTION E22B V12B V21B G12B AOPT 𝐸22𝑏, for bending behavior. 𝜈12𝑏, for bending behavior. 𝜈21𝑏, for bending behavior. 𝐺12𝑏, for bending behavior. Material axes option : EQ.0.0: locally orthotropic with material axes determined by element nodes 1, 2, and 4, as with *DEFINE_COORDI- NATE_NODES, and then rotated about the shell ele- ment normal by the angle BETA. EQ.2.0: globally orthotropic with material axes determined by vectors defined below, as with *DEFINE_COORDI- NATE_VECTOR. EQ.3.0: locally orthotropic material axes determined by rotating the material axes about the element normal by an angle, BETA, from a line in the plane of the element defined by the cross product of the vector 𝐯 with the element normal. LT.0.0: the absolute value of AOPT is a coordinate system ID number (CID on *DEFINE_COORDINATE_NODES, *DEFINE_COORDINATE_SYSTEM or *DEFINE_CO- ORDINATE_VECTOR). Available in R3 version of 971 and later. LN11 LN22 LN12 LQ1 LQ2 LM11 LM22 LM12 Yield curve ID for 𝑁11, the in-plane force resultant. Yield curve ID for 𝑁22, the in-plane force resultant. Yield curve ID for 𝑁12, the in-plane force resultant. Yield curve ID for 𝑄1, the transverse shear resultant. Yield curve ID for 𝑄2, the transverse shear resultant. Yield curve ID for 𝑀11, the moment. Yield curve ID for 𝑀22, the moment. Yield curve ID for 𝑀12, the moment. *MAT_RESULTANT_ANISOTROPIC DESCRIPTION A1, A2, A3 (𝑎1, 𝑎2, 𝑎3), define components of vector 𝐚 for AOPT = 2. V1, V2, V3 (𝑣1, 𝑣2, 𝑣3), define components of vector 𝐯 for AOPT = 3. D1, D2, D3 (𝑑1, 𝑑2, 𝑑3), define components of vector 𝐝 for AOPT = 2. BETA Material angle in degrees for AOPT = 0 and 3, may be overridden on the element card, see *ELEMENT_SHELL_BETA. Remarks: The in-plane elastic matrix for in-plane, plane stress behavior is given by: 𝐂in plane = 𝑄11𝑝 𝑄12𝑝 0 0 0 ⎤ 𝑄12𝑝 𝑄22𝑝 0 0 0 ⎥ ⎥ 0 0 𝑄44𝑝 0 0 ⎥ ⎥ 0 0 0 𝑄55𝑝 0 ⎥ 0 0 0 0 𝑄66𝑝⎦ ⎡ ⎢ ⎢ ⎢ ⎢ ⎢ ⎣ The terms 𝑄𝑖𝑗𝑝 are defined as: 𝑄11𝑝 = 𝑄22𝑝 = 𝑄12𝑝 = 𝐸11𝑝 1 − 𝜈12𝑝𝜈21𝑝 𝐸22𝑝 1 − 𝜈12𝑝𝜈21𝑝 𝜈12𝑝𝐸11𝑝 1 − 𝜈12𝑝𝜈21𝑝 𝑄44𝑝 = 𝐺12𝑝 𝑄55𝑝 = 𝐺23𝑝 𝑄66𝑝 = 𝐺31𝑝 The elastic matrix for bending behavior is given by: 𝐂bending = 𝑄11𝑏 𝑄12𝑏 0 ⎤ ⎡ 𝑄12𝑏 𝑄22𝑏 0 ⎥ ⎢ 0 0 𝑄44𝑏⎦ ⎣ The terms 𝑄𝑖𝑗𝑝 are similarly defined. Because this is a resultant formulation, no stresses are output to d3plot, and forces and moments are reported to elout in place of stresses. *MAT_STEEL_CONCENTRIC_BRACE This is Material Type 171. It represents the cyclic buckling and tensile yielding behavior of steel braces and is intended primarily for seismic analysis. Use only for beam elements with ELFORM = 2 (Belytschko-Schwer beam). Card 1 1 Variable MID 2 RO 3 YM Type A8 F F 4 PR F 5 6 7 8 SIGY LAMDA FBUCK FBUCK2 F F F F Default none none none none none See Remarks See Remarks 0.0 Card 2 1 2 3 4 5 6 7 8 Variable CCBRF BCUR Type F F Default See Remarks Card 3 1 2 3 4 5 6 7 8 Variable TS1 TS2 TS3 TS4 CS1 CS2 CS3 CS4 Type Default F 0 F 0 F 0 F 0 F F F F = TS1 = TS2 = TS3 = TS4 VARIABLE MID DESCRIPTION Material identification. A unique number or label not exceeding 8 characters must be specified. RO Mass density VARIABLE DESCRIPTION YM PR Young’s Modulus Poisson’s Ratio SIGY Yield stress LAMDA Slenderness ratio (optional – see note) FBUCK Initial buckling load (optional – see note. If used, should be positive) FBUCK2 Optional extra term in initial buckling load – see note CCBRF Reduction factor on initial buckling load for cyclic behavior BCUR Optional load curve giving compressive buckling load (y-axis) versus compressive strain (x-axis - both positive) TS1 - TS4 Tensile axial strain thresholds 1 to 4 CS1 - CS4 Compressive axial strain thresholds 1 to 4 Remarks: The brace element is intended to represent the buckling, yielding and cyclic behavior of steel elements such as tubes or I-sections that carry only axial loads. Empirical relationships are used to determine the buckling and cyclic load-deflection behavior. A single beam element should be used to represent each structural element. The cyclic behavior is shown in the graph (compression shown as negative force and displacement). 16 17 15 12 19 14 11,13 10 18 Figure M171-1. The initial buckling load (point 2) is: 𝐹𝑏 initial = FBUCK + FBUCK2 𝐿2 where FBUCK, FBUCK2 are input parameters and L is the length of the beam element. If neither FBUCK nor FBUCK2 are defined, the default is that the initial buckling load is where A is the cross sectional area. The buckling curve (shown dashed) has the form: SIGY × A, 𝐹(𝑑) = 𝐹b initial √𝐴𝛿 + 𝐵 where 𝛿 is abs(strain/yield strain), and A and B are internally-calculated functions of slenderness ratio (λ) and loading history. The member slenderness ratio λ is defined as 𝑘𝐿 𝑟 , where k depends on end conditions, L is the element length, and r is the radius of gyration such that 𝐴𝑟2 = 𝐼 (and 𝐼 = min(𝐼𝑦𝑦, 𝐼𝑧𝑧)); λ will by default be calculated from the section properties and element length using k = 1. Optionally, this may be overridden by input parameter LAMDA to allow for different end conditions. Optionally, the user may provide a buckling curve BCUR. The points of the curve give compressive displacement (x-axis) versus force (y-axis); the first point should have zero displacement and the initial buckling force. Displacement and force should both be positive. The initial buckling force must not be greater than the yield force. The tensile yield force (point 5 and section 16-17) is defined by 𝐹𝑦 = SIGY × 𝐴, where yield stress SIGY is an input parameter and A is the cross-sectional area. Following initial buckling and subsequent yield in tension, the member is assumed to be damaged. The initial buckling curve is then scaled by input parameter CCBRF, leading to reduced strength curves such as segments 6-7, 10-14 and 18-19. This reduction factor is typically in the range 0.6 to 1.0 (smaller values for more slender members). By default, CCBRF is calculated using SEAOC 1990: CCBRF = ⎜⎜⎜⎛1 + 0.5𝜆 𝜋√ ⎟⎟⎟⎞ 0.5𝜎𝑦⎠ ⎝ When tensile loading is applied after buckling, the member must first be straightened before the full tensile yield force can be developed. This is represented by a reduced unloading stiffness (e.g. segment 14-15) and the tensile reloading curve (segments 8-9 and 15-16). Further details can be found in Bruneau, Uang, and Whittaker [1998] and Structural Engineers Association of California [1974, 1990, 1996]. Solid line: λ = 25 (stocky) Dashed line: (slender) λ = 120 Figure M171-2. The response of stocky (low λ) and slender (high λ) braces are compared in the graph. These differences are achieved by altering the input value LAMDA (or the section properties of the beam) and FBUCK. *MAT_STEEL_CONCENTRIC_BRACE Axial Strain and Internal Energy may be plotted from the INTEGRATED beam results menus in Oasys Ltd. Post processors: D3PLOT and T/HIS. FEMA thresholds are the total axial strains (defined by change of length/initial length) at which the element is deemed to have passed from one category to the next, e.g. “Elastic”, “Immediate Occupancy”, “Life Safe”, etc. During the analysis, the maximum tensile and compressive strains (“high tide strains”) are recorded. These are checked against the user-defined limits TS1 to TS4 and CS1 to CS4. The output flag is then set to 0, 1, 2, 3, or 4 according to which limits have been passed. The value in the output files is the highest such flag from tensile or compressive strains. To plot this data, select INTEGRATED beam results, Integration point 4, Axial Strain. Maximum plastic strains in tension and compression are also output. These are defined as maximum total strain to date minus the yield or first buckling strain for tensile and compressive plastic strains respectively. To plot these, select INTEGRATED beam results, Integration point 4, “shear stress XY” and “shear stress XZ” for tensile and compressive plastic strains, respectively. *MAT_172 This is Material Type 172, for shell and Hughes-Liu beam elements only. The material model can represent plain concrete only, reinforcing steel only, or a smeared combination of concrete and reinforcement. The model includes concrete cracking in tension and crushing in compression, and reinforcement yield, hardening and failure. Properties are thermally sensitive; the material model can be used for fire analysis. Material data and equations governing the behavior (including thermal properties) are taken from Eurocode 2 (EC2). See notes below for more details of how the standard is applied in the material model. Although the material model offers many options, a reasonable response may be obtained by entering only RO, FC and FT for plain concrete; if reinforcement is present, YMREINF, SUREINF, FRACRX, FRACRY must be defined. Note that, from release R10 onwards, the number of possible cracks has been increased from 2 (0 and 90 degrees) to 4 – see notes below. NOTE: This material does not support specification of a ma- terial angle, 𝛽𝑖, for each through-thickness integra- tion point of a shell. Card 1 1 Variable MID 2 RO Type A8 F 3 FC F 4 FT F 5 6 7 8 TYPEC UNITC ECUTEN FCC F F F F Default none none none 0.0 1.0 1.0 0.0025 FC Card 2 1 2 3 4 5 6 7 8 Variable ESOFT LCHAR MU TAUMXF TAUMXC ECRAGG AGGSZ UNITL Type F F F F F F F F Default See notes 0.0 0.4 1020 1.161 × FT 0.001 0.0 1.0 Card 3 1 2 3 4 5 6 7 8 Variable YMREINF PRREINF SUREINF TYPER FRACRX FRACY LCRSU LCALPS Type F F F F F F I I Default none 0.0 0.0 1.0 0.0 0.0 none none Card 4 1 2 3 4 5 6 7 8 Variable AOPT ET36 PRT36 ECUT36 LCALPC DEGRAD ISHCHK UNLFAC Type F F F F I F Default 0.0 0.0 0.25 1020 none 0.0 Additional card for AOPT > 0. Card 5 Variable 1 XP Type F 2 YP F 3 ZP F 4 A1 F 5 A2 F 6 A3 F Default 0.0 0.0 0.0 0.0 0.0 0.0 I 0 F 0.5 7 8 Additional card for AOPT > 0. Card 6 Variable 1 V1 Type F 2 V2 F 3 V3 F 4 D1 F 5 D2 F 6 D3 F 7 8 BETA F Default 0.0 0.0 0.0 0.0 0.0 0.0 0.0 Omit if ISHCHK = 0 Card 7 1 2 3 4 5 6 7 8 Variable TYPSEC P_OR_F EFFD GAMSC ERODET ERODEC ERODER TMPOFF Type F F F F F F F F Default 0.0 0.0 0.0 0.0 2.0 0.01 0.05 0.0 Additional card for TYPEC = 6 or 9. Card 8 1 2 3 4 5 6 7 8 Variable ECI_6 ECSP69 GAMCE9 PHIEF9 Type F F F F Default see notes see notes 0.0 0.0 Define this card only if FT is negative. Card 9 1 2 3 4 5 6 7 8 Variable FT2 FTSHR LCFTT WRO_G ZSURF Type F F F F F Default abs(FT) abs(FT2) 0.0 0.0 0.0 VARIABLE DESCRIPTION MID RO FC Material identification. A unique number or label not exceeding 8 characters must be specified. Mass density Compressive strength of concrete (stress units). depends on TYPEC. Meaning TYPEC = 1,2,3,4,5,7,8: FC is the actual compressive strength TYPEC = 6: TYPEC = 9: is FC strength used in Mander equations. the unconfined compressive FC is the characteristic compressive strength (fck in EC2 1-1). See also FCC and the notes below. FT Tensile stress to cause cracking. Negative value to read card 9. TYPEC Concrete relationships aggregate type for stress-strain-temperature EQ.1.0: Siliceous (default), Draft EC2 Annex (fire engineering) EQ.2.0: Calcareous, Draft EC2 Annex (fire engineering) EQ.3.0: Non-thermally-sensitive using ET3, ECU3 EQ.4.0: Lightweight EQ.5.0: Fiber-reinforced EQ.6.0: Non-thermally-sensitive, Mander algorithm EQ.7.0: Siliceous, EC2 1-2:2004 (fire engineering) EQ.8.0: Calcareous, EC2 1-2:2004 (fire engineering) EQ.9.0: EC2 1-1:2004 (general and buildings) To obtain the pre-R9 behaviour, i.e. maximum of 2 cracks, add 100 to TYPEC. For example, 109 means 2 cracks, EC2 1-1:2004 (general and buildings). VARIABLE UNITC DESCRIPTION Factor to convert stress units to MPa (used in shear capacity checks and for application of EC2 formulae when TYPEC = 9) e.g. if model units are Newtons and metres, UNITC=10^-6. ECUTEN Strain to fully open a crack. FCC Relevant only if TYPEC = 6 or 9. TYPEC = 6: FCC is the compressive strength of confined concrete used in Mander equations. Default: un- confined properties are assumed. TYPEC = 9: FCC is the actual compressive strength. If blank, this will be set equal to the mean compres- sive strength (fcm in EC2 1-1) as required for ser- viceability calculations (8MPa greater than FC). For ultimate load calculations the user may set FCC to a factored characteristic compressive strength. See notes below. ESOFT Tension stiffening (Slope of stress-strain curve post-cracking in tension) MU Friction on crack planes (max shear = 𝜇 × compressive stress) TAUMXF TAUMXC ECRAGG AGGSZ UNITL Maximum friction shear stress on crack planes (ignored if AGGSZ > 0 - see notes). Maximum through-thickness shear stress after cracking . Strain parameter for aggregate interlock (ignored if AGGSZ > 0 - see notes). Aggregate size (length units - used in NS3473 aggregate interlock formula - see notes). Factor to convert length units to millimeters (used only if AGGSZ > 0 if model unit is meters, UNITL = 1000. - see notes) e.g. LCHAR Characteristic length at which ESOFT applies, also used as crack spacing in aggregate-interlock calculation *MAT_CONCRETE_EC2 DESCRIPTION YMREINF Young’s Modulus of reinforcement PRREINF Poisson’s Ratio of reinforcement SUREINF Ultimate stress of reinforcement TYPER Type of reinforcement for stress-strain-temperature relationships EQ.1.0: Hot rolled reinforcing steel, Draft EC2 Annex (fire) EQ.2.0: Cold worked reinforcing steel (default), Draft EC2 Annex (fire) EQ.3.0: Quenched/tempered prestressing steel, Draft EC2 Annex (fire) EQ.4.0: Cold worked prestressing steel, Draft EC2 Annex (fire) EQ.5.0: Non-thermally sensitive using loadcurve LCRSU. EQ.7.0: Hot rolled reinforcing steel, EC2 1-2:2004 (fire) EQ.8.0: Cold worked reinforcing steel, EC2 1-2:2004 (fire) Fraction of reinforcement (𝑥-axis). For example, to obtain 1% reinforcement set FRACR = 0.01. Fraction of reinforcement (𝑦-axis). For example, to obtain 1% reinforcement set FRACR = 0.01. Loadcurve for TYPER = 5, giving non-dimensional factor on SUREINF versus plastic stress-strain relationships from EC2). (overrides strain FRACRX FRACRY LCRSU LCALPS Optional loadcurve giving thermal expansion coefficient of reinforcement vs temperature – overrides relationship from EC2. VARIABLE AOPT DESCRIPTION Material axes option : EQ.0.0: locally orthotropic with material axes determined by element nodes 1, 2, and 4, as with *DEFINE_COORDI- NATE_NODES, and then rotated about the shell ele- ment normal by an angle BETA. EQ.2.0: globally orthotropic with material axes determined by vectors defined below, as with *DEFINE_COORDI- NATE_VECTOR. EQ.3.0: locally orthotropic material axes determined by rotating the material axes about the element normal by an angle, BETA, from a line in the plane of the element defined by the cross product of the vector 𝐯 with the element normal. LT.0.0: This option has not yet been implemented for this material model. ET36 Young’s Modulus of concrete (TYPEC = 3 and 6). For other values of TYPEC, the Young’s Modulus is calculated internally: see notes. PRT36 Poisson’s Ratio of concrete (TYPEC = all). ECUT36 Strain to failure of concrete in compression (TYPEC = 3 and 6). LCALPC DEGRAD ISHCHK Optional loadcurve giving thermal expansion coefficient of concrete vs temperature – overrides relationship from EC2. If non-zero, the compressive strength of concrete parallel to an open crack will be reduced . Set this flag to 1 to input Card 7 (shear capacity check and other optional input data). UNLFAC Stiffness degradation factor after crushing (0.0 to 1.0 – see notes). XP, YP, ZP Not used. A1, A2, A3 Components of vector 𝐚 for AOPT = 2. V1, V2, V3 Components of vector 𝐯 for AOPT = 3. D1, D2, D3 Components of vector 𝐝 for AOPT = 2. BETA *MAT_CONCRETE_EC2 DESCRIPTION Material angle in degrees for AOPT = 0 and AOPT = 3. BETA may be overridden on the element card, see *ELEMENT_- SHELL_BETA TYPESC Type of shear capacity check EQ.1.0: BS 8110 EQ.2.0: ACI P_OR_F EFFD If BS8110 shear check, percent reinforcement – e.g. if 0.5%, input 0.5. If ACI shear check, ratio (cylinder strength/FC) - defaults to 1. Effective section depth (length units), used in shear capacity check. This is usually the section depth excluding the cover concrete. GAMSC Load factor used in BS8110 shear capacity check. ERODET Crack-opening strain at which element is deleted ERODEC Compressive strain used in erosion criteria, see notes ERODER Reinforcement plastic strain used in erosion criteria, see notes TMPOFF Constant to be added to the model’s temperature unit to convert into degrees Celsius, e.g., if the model’s temperature unit is Degrees Celsius degrees Kelvin, set TMPOFF temperatures are then used throughout the material model, e.g., for LCALPC as well as for the default thermally-sensitive properties. -273. to EC1_6 Strain at maximum compressive stress for Type 6 concrete. ECSP69 Spalling strain in compression for TYPEC = 6 and 9. GAMCE9 Material factor that divides the Youngs Modulus (TYPEC = 9). PHIEF9 Effective creep ratio (TYPEC = 9). FT2 Tensile strength used for calculating tensile response. FTSHR Tensile strength used for calculating post-crack shear response. LCFTT Loadcurve defining factor on tensile strength versus time. VARIABLE DESCRIPTION WRO_G Density times gravity for water pressure in cracks ZSURF Z-coordinate of water surface (for water pressure in cracks) Remarks: reinforced concrete with evenly distributed This material model can be used to represent unreinforced concrete (FRACR = 0), steel (FRACR = 1), or reinforcement (0 < FRACR < 1). Concrete is modelled as an initially-isotropic material with a non- rotating smeared crack approach in tension, together with a plasticity model for compressive loading. Reinforcement is treated as separate sets of bars in the local element x and y axes. The reinforcement is assumed not to carry through-thickness shear or in-plane shear. Therefore, this material model should not be used to model steel-only sections, i.e. do not create a section in which all the integration points are of *MAT_172 with FRACRX, FRACRY = 1. Creating Reinforced Concrete Sections: Reinforced concrete sections for shell or beam elements may be created using *PART_ COMPOSITE (for shells) or *INTEGRATION_BEAM (for beams) to define the section. Create one Material definition representing the concrete using MAT_CONCRETE_EC2 with FRACR = 0. Create another Material definition representing the reinforcement using MAT_CONCRETE_EC2 with FRACRX and/or FRACRY = 1. The Material ID of each integration point is then set to represent either concrete or steel. The position of each integration point within the cross-section and its cross-sectional area are chosen to represent the actual distribution of reinforcement. Options for TYPEC and TYPER Eurocode 2 (EC2) contains different sections applicable to general structural engineering versus fire engineering. The latter contains different data for different types of concrete and steel, and has been revised during its history. TYPEC and TYPER control the version and section of the EC2 document from which the material data is taken, and the types of concrete and steel being represented. In the descriptions of TYPEC and TYPER above, “Draft EC2 Annex (fire engineering)” means data taken from the 1995 draft Eurocode 2 Part 1-2 (for fire engineering), ENV 1992-1-2:1995. These are the defaults, and are suitable for general use where elevated temperatures are not considered. EC2 was then issued in 2004 (described above as EC2 1-2:2004 (fire)) with revised stress- strain data at elevated temperatures (TYPEC and TYPER = 7 or 8). These settings are recommended for analyses with elevated temperatures. Meanwhile Eurocode 2 Part 1-1 (for general structural engineering), EC2 1-1:2004, contains material data and formulae that differ from Part 1-2; these are obtained by setting TYPEC = 9. This setting is recommended where compatibility is required with the structural engineering data and assumptions of Part 1-1 of the Eurocode. A further option for modelling concrete, TYPEC = 6, is provided for applications such as seismic engineering in which the different stress-strain behaviors of confined versus unconfined concrete needs to be captured. This option uses equations by Mander et al, and does not relate directly to Eurocode 2. Material Behavior: Concrete Thermal sensitivity For TYPEC = 1,2,4,5,7,8, the material properties are thermally-sensitive. If no temperatures are defined in the model, it behaves as if at 20degC. Pre-programmed relationships between temperature and concrete properties are taken from the EC2 document. The thermal expansion coefficient is as defined in EC2, is non-zero by default, and is a function of temperature. This may be overridden by inputting the curve LCALPC. TYPEC = 3, 6 and 9 are not thermally sensitive and have no thermal expansion coefficient by default. Tensile response The concrete is assumed to crack in tension when the maximum in-plane principal stress reaches FT. A non-rotating smeared crack approach is used. Cracks can open and close repeatedly under hysteretic loading. When a crack is closed it can carry compression according to the normal compressive stress-strain relationships. The direction of the crack relative to the element coordinate system is stored when the crack first forms. The material can carry compression parallel to the crack even when the crack is open. Further cracks may then form at pre-determined angles to the first crack, if the tensile stress in that direction reaches FT. In versions up to R9.0, the number of further cracks is limited to one, at 90 degrees to the first crack. In versions starting from R10, up to three further cracks can form, at 45, 90 amd 135 degrees to the first crack. The tensile stress is limited to FT only in the available crack directions. The tensile stress in other directions is unlimited, and could exceed FT. This is a limitation of the non-rotating crack approach and may lead to models being non-conservative, i.e. the response is stronger than implied by the input. The increase of the possible number of cracks from two to four significantly reduces this error, and may therefore cause models to seem “weaker” in R10 than in R9 under some loading conditions. An option to revert to the previous 2-crack behaviour is available in R10 – add 100 to TYPEC. After initial cracking, the tensile stress reduces with increasing tensile strain. A finite amount of energy must be absorbed to create a fully open crack - in practice the reinforcement holds the concrete together, allowing it to continue to take some tension (this effect is known as tension-stiffening). The options available for the stress-strain relationship are shown below. The bilinear relationship is used by default. The simple linear relationship applies only if ESOFT > 0 and ECUTEN = 0. Figure M172-1. Tensile Behaviour of Concrete LCHAR can optionally be used to maintain constant energy per unit area of crack irrespective of mesh size, i.e. the crack opening displacement is fixed rather than the crack opening strain. LCHAR × ECUTEN is then the displacement to fully open a crack. For the actual elements, crack opening displacement is estimated by strain × √area. Note that if LCHAR is defined, it is also used as the crack spacing in the NS 3473 aggregate interlock calculation. For the thermally-sensitive values of TYPEC, the relationship of FT with temperature is taken from EC2 – there is no input option to change this. FT is assumed to remain at its input value at temperatures up to 100°C, then to reduce linearly with temperature to zero at 600°C. Up to 500°C, the crack opening strain ECUTEN increases with temperature such that the fracture energy to open the crack remains constant. Above 500 deg C the crack opening strain does not increase further. In some concrete design codes and standards, it is stipulated that the tensile strength of concrete should be assumed to be zero. However, for MAT_CONCRETE_EC2 it is not recommended to set FT to zero, because: •Cracks will form at random orientations caused by small dynamic tensile stresses, leading to unexpected behavior when the loading increases because the crack orientations are fixed when the cracks first form; •The shear strength of cracked concrete may then also become zero in the analysis (according to the aggregate interlock formula, the post-crack shear strength is assumed proportional to FT). These problems may be tackled by using the inputs on Card 9. Firstly, separate tensile strengths may be input for the tensile response and for calculating the shear strength of cracked concrete. Secondly, by using the loadcurve LCFTT, the tensile strength may be ramped gradually down to zero after the static loads have been applied, ensuring that the cracks will form in the correct orientation Compressive response: TYPEC = 1,2,4,5,7,8 For TYPEC = 1,2,4,5,7,8, the compressive behavior of the concrete initially follows a stress-strain curve defined in EC2 as: Stress = FCmax × ) × 𝜀cl ⎡( ⎢ ⎣ 2 + ( 𝜀 𝜀cl ) ⎤ ⎥ ⎦ where 𝜀cl is the strain at which the ultimate compressive strength FCmax is reached, and 𝜀 is the current equivalent uniaxial compressive strain. The initial elastic modulus is given by 𝐸 = 3 × FCmax/2𝜀cl. On reaching FCmax, the stress decreases linearly with increasing strain, reaching zero at a strain 𝜀cu. Strains 𝜀cl and 𝜀cu are by default taken from EC2 and are functions of temperature. At 20oC they take values 0.0025 and 0.02 respectively. FCmax is also a function of temperature, given by the input parameter FC (which applies at 20oC) times a temperature-dependent softening factor taken from EC2. The differences between TYPEC = 1,2,4,5,7,8 are limited to (a) different reductions of FC at elevated temperatures, and (b) different values of 𝜀cl at elevated temperatures. Figure M172-2. Concrete stress strain behavior Compressive response: TYPEC = 3 For TYPEC = 3, the user over-rides the default values of Young’s Modulus and 𝜀cu using ET36 and ECUT36 respectively. In this case, the strain 𝜀cl is calculated from the elastic stiffness, and there is no thermal sensitivity. The stress-strain behaviour follows the same form as described above. Compressive response: TYPEC = 6 For TYPEC = 6, the above compressive crushing behaviour is replaced with the equations proposed by Mander. This algorithm can model unconfined or confined concrete; for unconfined, leave FCC blank. For confined concrete, input the confined compressive strength as FCC. Figure M172-3. Type 6 concrete Default values for type 6 are calculated as follows: 𝜀cl = 0.002 × [1 + 5 ( FCC6 FC − 1)] 𝜀cu = 1.1 × 𝜀c 𝜀csp = 𝜀cu + 2 FCC Note that for unconfined concrete, FCC6 = FC causing 𝜀cl to default to 0.002. Compressive response: TYPEC = 9 For TYPEC = 9, the input parameter FC is the characteristic cylinder strength in the stress units of the model. FC x UNITC is assumed to be fck, the strength class in MPa units. The mean tensile strength fctm, mean Young’s Modulus Ecm, and the strains used to construct the stress-strain curve such as 𝜀cl are by default evaluated automatically from tabulated functions of fck given in Table 3.1 of EC2. The compressive strength of the material is given by the input parameter FCC, which defaults to the mean compressive strength fcm defined in EC2 as fck + 8MPa). The user may override the default compressive strength by inputting FCC explicitly. The stress-strain curve follows this form: 𝑆𝑡𝑟𝑒𝑠𝑠 𝐹𝐶𝐶 = 𝑘𝜂 − 𝜂2 1 + (𝑘 − 2)𝜂 Where FCC is the input parameter FCC (default: = (fck + 8MPa)/UNITC), 𝜼 = 𝒔𝒕𝒓𝒂𝒊𝒏/𝜺cl, 𝒌 = 𝟏. 𝟎𝟓𝑬 × 𝜺𝒄𝟏 𝑭𝑪𝑪⁄ E is the Young’s Modulus. The default parameters are intended to be appropriate for a serviceability analysis (mean properties), so default FT = fctm and default E = Ecm. For an ultimate load analysis, FCC should be the “design compressive strength” (normally the factored characteristic strength, including any appropriate material factors); FT should be input as the factored characteristic tensile strength; GAMCE9 may be input (a material factor that divides the Young’s Modulus so E = Ecm/GAMCE9); and a creep factor PHIEF9 may be input: this scales 𝜺cl by (1+PHIEF9). Unload/reload stiffness (all concrete types): During compressive loading, the elastic modulus will be reduced according to the parameter UNLFAC (default = 0.5). UNLFAC = 0.0 means no reduction, i.e. the initial elastic modulus will apply during unloading and reloading. UNLFAC = 1.0 means that unloading results in no permanent strain. Intermediate values imply a permanent strain linearly interpolated between these extremes. Figure M172-4. Concrete unloading behavior Tensile strength is reduced by the same factor as the elastic modulus as described in the paragraph above. Optional compressive strength degradation due to cracking: By default, the compressive strength of cracked and uncracked elements is the same. If DEGRAD is non-zero, the formula from BS8110 is used to reduce compressive strength parallel to the crack while the crack is open: Reduction factor = min (1.0, 1.0 0.8 + 100𝜀𝑡 ) , where 𝜀𝑡 is the tensile strain normal to the crack. Shear strength on crack planes: Before cracking, the through-thickness shear stress in the concrete is unlimited. For cracked elements, shear stress on the crack plane (magnitude of shear stress including element-plane and through-thickness terms) is treated in one of two ways: 1. If AGGSZ > 0, the relationship from Norwegian standard NS3473 is used to model the aggregate-interlock that allows cracked concrete to carry shear load- ing. In this case, UNITL must be defined. This is the factor that converts model length units to millimetres, i.e. the aggregate size in millimetres = AGGSZ × UNITL. The formula in NS3473 also requires the crack width in millimetres: this is estimated from UNITL × 𝜀cro × 𝐿𝑒, here 𝜀cro is the crack opening strain and 𝐿𝑒 is the crack spacing, taken as LCHAR if non-zero, or equal to element size if LCHAR is zero. Optionally, TAUMXC may be used to set the maximum shear stress when the crack is closed and the normal stress is zero – by default this is equal to 1.161FT from the formulae in NS3473. If TAUMXC is defined, the shear stress from the NS3473 formula is scaled by TAUMXC / 1.161FT. 2. If AGGSZ = 0, the aggregate interlock is modeled by this formula: 𝜏max = TAUMXC 𝜀cro ECRAGG 1.0 + + min(MU × 𝜎comp,TAUMXF) Where 𝜏max is the maximum shear stress carried across a crack; 𝜎compis the compressive stress across the crack (this is zero if the crack is open); ECRAGG is the crack opening strain at which the input shear strength TAUMXC is halved. Again, TAUMXC defaults to 1.161FT. Note that if a shear capacity check is specified, the above applies only to in-plane shear, while the through-thickness shear is unlimited. Reinforcement The reinforcement is treated as separate bars providing resistance only in the local 𝑥 and 𝑦 directions – it does not carry shear in-plane or out of plane. For TYPER = 1,2,3,4,7,8, the behaviour is thermally sensitive and follows stress-strain relationships of a form defined in EC2. At 20oC (or if no thermal input is defined) the behaviour is elastic-perfectly-plastic with Young’s Modulus EREINF and ultimate stress SUREINF, up to the onset of failure, after which the stress reduces linearly with increasing strain until final failure. At elevated temperatures there is a nonlinear transition between the elastic phase and the perfectly plastic phase, and EREINF and SUREINF are scaled down by temperature-dependent factors defined in EC2. The strain at which failure occurs depends on the reinforcement type (TYPER) and the temperature. For example, for hot-rolled reinforcing steel at 20oC failure begins at 15% strain and is complete at 20% strain. The thermal expansion coefficient is as defined in EC2 and is a function of temperature. This may be overridden by inputting the curve LCAPLS. The differences between TYPER = 1,2,4,7,8 are limited to (a) different reductions of EREINF and SUREINF at elevated temperatures, (b) different nonlinear transitions between elastic and plastic phases and (c) the strains at which softening begins and is complete. The default stress-strain curve for reinforcement may be overridden using TYPER = 5 and LCRSU. In this case, the reinforcement properties are not temperature-sensitive and the yield stress is given by SUREINF × 𝑓 (𝜀𝑝), where 𝑓 (𝜀𝑝) is the loadcurve value at the current plastic strain. To include failure of the reinforcement, the curve should reduce to zero at the desired failure strain and remain zero for higher strains. Note that by default LS-DYNA re-interpolates the input curve to have 100 equally-spaced points; if the last point on the curve is at very high strain, then the initial part of the curve may become poorly defined. Local directions: AOPT and associated data are used to define the directions of the reinforcement bars. If the reinforcement directions are not consistent across neighbouring elements, the response may be less stiff than intended – this is equivalent to the bars being bent at the element boundaries. See material type 2 for description of the different AOPT settings. Shear capacity check: Shear reinforcement is not included explicitly in this material model. However, a shear capacity check can be made, to show regions that require shear reinforcement. The assumption is that the structure will not yield or fail in through-thickness shear, because sufficient shear reinforcement will be added. Set ISHCHK and TYPESC to 1. Give the percentage reinforcement (P_OR_F), effective depth of section EFFD (this typically excludes the cover concrete), and load factor GAMSC. These are used in Table 3.8 of BS 8110-1:1997 to determine the design shear stress. The “shear capacity” is this design shear stress times the total section thickness (i.e. force per unit width), modified according to Equation 6b of BS 8110 to allow for axial load. The “shear demand” (actual shear force per unit width) is then compared to the shear capacity. This process is performed for the two local directions of the reinforcement in each element; when defining sections using integration rules and multiple sets of material properties, it is important that each set of material properties referenced within the same section has the same AOPT and orientation data. Note that the shear demand and axial load (used in calculation of the shear capacity) are summed across the integration points within the section; the same values of capacity, demand, and difference between capacity and demand are then written to all the integration points. *MAT_CONCRETE_EC2 By default, thermal expansion properties from EC2 are used. If no temperatures are defined in the model, properties for 20deg C are used. For TYPEC = 3, 6 or 9, and TYPER = 5, there is no thermal expansion by default, and the properties do not vary with temperature. The user may override the default thermal expansion behaviour by defining curves of thermal expansion coefficient versus temperature (LCALPC, LCALPR). These apply no matter what types TYPEC and TYPER have been selected. Output: “Plastic Strain” is the maximum of the plastic strains in the reinforcement in the two local directions. Element deletion: Elements are deleted from the calculation when all of their integration points have reached the erosion criterion: Concrete crack opening strain > ERODET or Concrete compressive strain > εc_erode where εc_erode = ERODEC + εcsp with εcsp the strain at which the stress-strain relation falls to zero. Reinforcement plastic strain > εr_erode where = ERODER + εrsp with εrsp the strain at which the stress-strain relation falls to zero, or if LCRSU > 0 εrsp is assumed to be 2.0. If the material is smeared concrete/reinforcement, i.e. 0 < max(FRACRX, FRACRY) < 1, the erosion criteria must be met for both concrete and reinforcement before erosion can occur Extra history variables may be requested for shell elements (NEIPS on *DATABASE_- EXTENT_BINARY), which have the following meaning: Extra Variable 1: Current crack opening strain (if two cracks are present, max of the two) Extra Variable 2: Equivalent uniaxial strain for concrete compressive behaviour Extra Variable 3: Number of cracks (0, 1 or 2) Extra Variable 4: Temperature Extra Variable 5: Thermal strain Extra Variable 6: Current crack opening strain – first crack to form Extra Variable 7: Current crack opening strain – crack at 90 degrees to first crack Extra Variable 8: Max crack opening strain – first crack to form Extra Variable 9: Max crack opening strain – crack at 90 degrees to first crack Extra Variable 10: Maximum difference (shear demand minus capacity) that has occurred so far, in either of the two reinforcement directions Extra Variable 11: Maximum difference (shear demand minus capacity) that has occurred so far, in reinforcement 𝑥-direction Extra Variable 12: Maximum difference (shear demand minus capacity) that has occurred so far, in reinforcement 𝑦-direction Extra Variable 13: Current shear demand minus capacity, in reinforcement 𝑥- direction Extra Variable 14: Current shear demand minus capacity, in reinforcement 𝑦- direction Extra Variable 15: Current shear capacity 𝑉cx, in reinforcement 𝑥-direction Extra Variable 16: Current shear capacity 𝑉cy, in reinforcement 𝑦-direction Extra Variable 17: Current shear demand 𝑉x, in reinforcement 𝑥-direction Extra Variable 18: Current shear demand 𝑉y, in reinforcement 𝑦-direction Extra Variable 19: Maximum shear demand that has occurred so far, in reinforcement x-direction Extra Variable 20: Maximum shear demand) that has occurred so far, in reinforcement y-direction Extra Variable 21: Current strain in reinforcement (𝑥-direction) Extra Variable 22: Current strain in reinforcement (𝑦-direction) Extra Variable 23: Engineering shear strain (slip) across first crack Extra Variable 24: Engineering shear strain (slip) across second crack Extra Variable 25: 𝑥-stress in concrete (element local axes) Extra Variable 26: 𝑦-stress in concrete (element local axes) Extra Variable 27: 𝑥𝑦-stress in concrete (element local axes) Extra Variable 28: 𝑦𝑧-stress in concrete (element local axes) Extra Variable 29: 𝑥𝑧-Stress in concrete (element local axes) Extra Variable 30: Reinforcement stress (𝑎-direction) Extra Variable 31: Reinforcement stress (𝑏-direction) Extra Variable 32: Current shear demand 𝑉max Extra Variable 33: Maximum 𝑉max that has occurred so far Extra Variable 34: Current shear capacity 𝑉cθ Extra Variable 35: Excess shear: 𝑉max − 𝑉cθ Extra Variable 36: Maximum excess shear that has occurred so far In the above list 𝑉max is given by 𝑉max = √𝑉𝑥 2 2 + 𝑉𝑦 Where 𝑉𝑥 and 𝑉𝑦 is the shear demand reinforcement in 𝑥 and 𝑦 directions respectively. Additionally, 𝑉𝑐𝜃 = √ √√ ⎷ 𝑉max ) ( 𝑉𝑥 𝑉𝑐𝑥 + ( 𝑉𝑦 𝑉𝑐𝑦 ) where 𝑉𝑐𝑥, 𝑉𝑐𝑦 are the shear capacities in the 𝑥 and 𝑦 directions. Note that the concrete stress history variables are stored in element local axes irrespective of AOPT, i.e. local 𝑥 is always the direction from node 1 to node 2. The reinforcement stresses are in the reinforcement directions; these do take account of AOPT. MAXINT (shells) and/or BEAMIP (beams) on *DATABASE_EXTENT_BINARY may be set to the maximum number of integration points, so that results for all integration points can be plotted separately. *MAT_173 This is Material Type 173 for solid elements only, is intended to represent sandy soils and other granular materials. Joints (planes of weakness) may be added if required; the material then represents rock. The joint treatment is identical to that of *MAT_JOINT- ED_ROCK. Card 1 1 2 3 4 5 6 7 8 Variable MID RO GMOD RNU (blank) PHI CVAL PSI Type A8 F F F F F F Default 0.0 Card 2 1 2 3 4 5 6 7 8 Variable NOVOID NPLANES (blank) LCCPDR LCCPT LCCJDR LCCJT LCSFAC Type Default 1 0 Card 3 1 I 0 2 3 I 0 4 I 0 5 I 0 6 I 0 7 I 0 8 Variable GMODDP GMODGR LCGMEP LCPHIEP LCPSIEP LCGMST CVALGR ANISO Type F F F F F F F F Default 0.0 0.0 0.0 0.0 0.0 0.0 0.0 1.0 Plane Cards. Repeat for each plane (maximum 6 planes). Card 4 1 2 3 4 5 6 7 8 Variable DIP DIPANG CPLANE FRPLANE TPLANE SHRMAX LOCAL Type F F F F F F F Default 0.0 0.0 0.0 0.0 0.0 1.e20 0.0 VARIABLE MID DESCRIPTION Material identification. A unique number or label not exceeding 8 characters must be specified. RO Mass density GMOD Elastic shear modulus RNU PHI Poisson’s ratio Angle of friction (radians) CVAL Cohesion value (shear strength at zero normal stress) PSI Dilation angle (radians) NOVOID Flag = 1 to switch off voiding behavior NPLANES Number of joint planes (maximum 6) LCCPDR Load curve for extra cohesion for parent material (dynamic relaxation) LCCPT Load curve for extra cohesion for parent material (transient) LCCJDR Load curve for extra cohesion for joints (dynamic relaxation) LCCJT Load curve for extra cohesion for joints (transient) LCSFAC Load curve giving factor on strength vs. time GMODDP Z-coordinate at which GMOD and CVAL are correct GMODGR Gradient of GMOD versus z-coordinate (usually negative) VARIABLE DESCRIPTION LCGMEP Load curve of GMOD versus plastic strain (overrides GMODGR) LCPHIEP Load curve of PHI versus plastic strain LCPSIEP Load curve of PSI versus plastic strain LCGMST (Leave blank) CVALGR Gradient of CVAL versus z-coordinate (usually negative) ANISO Factor applied to elastic shear stiffness in global XZ and YZ planes DIP Angle of the plane in degrees below the horizontal DIPANG Plan view angle (degrees) of downhill vector drawn on the plane CPLANE Cohesion for shear behavior on plane PHPLANE Friction angle for shear behavior on plane (degrees) TPLANE Tensile strength across plane (generally zero or very small) SHRMAX Max shear stress on plane (upper compression) limit, independent of LOCAL EQ.0: DIP and DIPANG are with respect to the global axes EQ.1: DIP and DIPANG are with respect to the local element axes Remarks: 1. The material has a Mohr Coulomb yield surface, given by τmax = C + σntan(PHI), where τmax = maximum shear stress on any plane, σn = normal stress on that plane (positive in compression), C = cohesion, PHI = friction angle. The plastic potential function is of the form βσk - σI + constant, where σk = maximum prin- cipal stress, σi = minimum principal stress, and 𝛽 = 1+sin(PSI) 1−sin(PSI). 2. The tensile strength of the material is given by 𝜎max = 𝐶 tan(PHI) where C is the cohesion. After the material reaches its tensile strength, further tensile straining leads to volumetric voiding; the voiding is reversible if the strain is reversed. 3. If depth-dependent properties are used, the model must be oriented with the z- axis in the upward direction. 4. Plastic strain is defined as √2 3 𝜀𝑝𝑖𝑗𝜀𝑝𝑖𝑗, i.e. the same way as for other elasto-plastic material models. 5. Friction and dilation angles PHI and PSI may vary with plastic strain, to model heavily consolidated materials under large shear strains – as the strain increas- es, the dilation angle typically reduces to zero and the friction angle to a lower, pre-consolidation value. 6. For similar reasons, the shear modulus may reduce with plastic strain, but this option may sometimes give unstable results. 7. The loadcurves LCCPDR, LCCPT, LCCJDR, LCCJT allow extra cohesion to be specified as a function of time. The cohesion is additional to that specified in the material parameters. This is intended for use during the initial stages of an analysis to allow application of gravity or other loads without cracking or yield- ing, and for the cracking or yielding then to be introduced in a controlled man- ner. This is done by specifying extra cohesion that exceeds the expected stresses initially, then declining to zero. If no curves are specified, no extra cohesion is applied. 8. The loadcurve for factor on strength applies simultaneously to the cohesion and tan(friction angle) of parent material and all joints. This feature is intended for reducing the strength of the material gradually, to explore factors of safety. If no curve is present, a constant factor of 1 is assumed. Values much greater than 1.0 may cause problems with stability. 9. The anisotropic factor ANISO applies the elastic shear stiffness in the global XZ It can be used only in pure Mohr-Coulomb mode and YZ planes. (NPLANES = 0). 10. For friction angle greater than zero, the Mohr Coulomb yield surface implies a tensile pressure limit equal to CVAL/tan(PHI). The default behaviour is that voids develop in the material when this pressure limit is reached, and the pres- sure will never become more tensile than the pressure limit. If NOVOID = 1, the tensile pressure limit is not applied. Stress states in which the pressure is more tensile than CVAL/tan(PHI) are permitted, but will be purely hydrostatic with no shear stress. NOVOID is recommended in Multi-Material ALE simula- tions, in which the development of voids or air space is already accounted for by the Multi-Material ALE. 11. To model soil, set NJOINT = 0. The joints are to allow modeling of rock, and are treated identically to those of *MAT_JOINTED_ROCK. 12. The joint plane orientations are defined by the angle of a “downhill vector” drawn on the plane, i.e. the vector is oriented within the plane to obtain the maximum possible downhill angle. DIP is the angle of this line below the hori- zontal. DIPANG is the plan-view angle of the line (pointing down hill) meas- ured clockwise from the global Y-axis about the global Z-axis. 13. Joint planes would generally be defined in the global axis system if they are taken from survey data. However, the material model can also be used to rep- resent masonry, in which case the weak planes represent the cement and lie parallel to the local element axes. 14. The joint planes rotate with the rigid body motion of the elements, irrespective of whether their initial definitions are in the global or local axis system. 15. Extra variables for plotting. By setting NEIPH on *DATABASE_EXTENT_BI- NARY to 27, the following variables can be plotted in Oasys Ltd. Post Proces- sors D3PLOT, T/HIS and LS-PrePost: Variable(s) Description 1 2 3 4 – 9 10 - 15 16 - 20 21 - 27 33 34 mobilized strength fraction for base material volumetric void strain maximum stress overshoot during plastic calculation crack opening strain for planes 1 - 6 crack accumulated engineering shear strain for planes 1 - 6 current shear utilization for planes 1 - 6 maximum shear utilization to date for planes 1 – 6 elastic shear modulus (for checking depth-dependent input) cohesion (for checking depth-dependent input) *MAT_RC_BEAM This is Material Type 174, for Hughes-Liu beam elements only. The material model can represent plain concrete only, reinforcing steel only, or a smeared combination of concrete and reinforcement. The main emphasis of this material model is the cyclic behavior – it is intended primarily for seismic analysis. Card 1 1 Variable MID 2 RO 3 EUNL Type A8 F F 4 PR F 5 FC F 6 7 8 EC1 EC50 RESID F F F Default none none See Remarks 0.0 none 0.0022 See Remarks 0.2 Card 2 Variable 1 FT 2 3 4 5 6 7 8 UNITC (blank) (blank) (blank) ESOFT LCHAR OUTPUT Type F F F F F F F Default See Remarks 1.0 none none none See Remarks none Card 3 1 2 3 4 5 6 7 F 0 8 Variable FRACR YMREIN PRREIN SYREIN SUREIN ESHR EUR RREINF Type F F F F F F F F Default 0.0 none 0.0 0.0 SYREIN 0.03 0.2 4.0 VARIABLE MID DESCRIPTION Material identification. A unique number or label not exceeding 8 characters must be specified. VARIABLE DESCRIPTION RO Mass density EUNL Initial unloading elastic modulus . PR FC EC1 EC50 Poisson’s ratio. Cylinder strength (stress units) Strain at which stress FC is reached. Strain at which the stress has dropped to 50% FC RESID Residual strength factor FT Maximum tensile stress UNITC Factor to convert stress units to MPa ESOFT Slope of stress-strain curve post-cracking in tension LCHAR Characteristic length for strain-softening behavior OUTPUT Output flag controlling what is written as “plastic strain” EQ.0.0: Curvature EQ.1.0: “High-tide” plastic strain in reinforcement FRACR Fraction of FRACR = 0.01) reinforcement (e.g. for 1% reinforcement YMREIN Young’s Modulus of reinforcement PRREIN Poisson’s Ratio of reinforcement SYREIN Yield stress of reinforcement SUREIN Ultimate stress of reinforcement ESHR EUR R_REINF Strain at which reinforcement begins to harden Strain at which reinforcement reaches ultimate stress Dimensionless Ramberg-Osgood parameter r. If zero, a default value r = 4.0 will be used. If set to -1, parameters will be calculated from Kent & Park formulae. Creating sections for reinforced concrete beams: This material model can be used to represent unreinforced concrete (FRACR = 0), steel reinforcement (FRACR = 1), or (0 < FRACR < 1). reinforced concrete with evenly distributed Alternatively, use *INTEGRATION_BEAM to define the section. A new option in allows the user to define a Part ID for each integration point, similar to the facility already available with *INTEGRATION_SHELL. All parts referred to by one integration rule must have the same material type, but can have different material properties. Create one Part for concrete, and another for steel. These Parts should reference Materials, both of type *MAT_RC_BEAM, one with FRACR = 0, the other with FRACR = 1. Then, by assigning one or other of these Part Ids to each integration point the reinforcement can be applied to the correct locations within the section of the beam. Concrete: In monotonic compression, the approach of Park and Kent, as described in Park & Paulay [1975] is used. The material follows a parabolic stress-strain curve up to a maximum stress equal to the cylinder strength FC; therafter the strength decays linearly with strain until the residual strength is reached. Default values for some material parameters will be calculated automatically as follows: EC50 = (3 + 0.29𝐹𝐶) 145𝐹𝐶 − 1000 where FC is in MPa as per Park and Kent test data. EUNL = initial tangent slope = 2FC EC1 User-defined values for EUNL lower than this are not permitted, but higher values may be defined if desired. FT = 1.4 ( FC 10 ) where FC is in MPa as per Park and Kent test data. ESOFT = EUNL User-defined values higher than EUNL are not permitted. UNITC is used only to calculate default values for the above parameters from FC. Strain-softening behavior tends to lead to deformations being concentrated in one element, and hence the overall force-deflection behavior of the structure can be mesh- size-dependent if the softening is characterized by strain. To avoid this, a characteristic length (LCHAR) may be defined. This is the length of specimen (or element) that would exhibit the defined monotonic stress-strain relationship. LS-DYNA adjusts the stress-strain relationship after ultimate load for each element, such that all elements irrespective of their length will show the same deflection during strain softening (i.e. between ultimate load and residual load). Therefore, although deformation will still be concentrated in one element, the load-deflection behavior should be the same irrespective of element size. For tensile behavior, ESOFT is similarly scaled. MAT_RC_BEAM - concrete 17 18 16 15,19 20 7 7,9 5,12 8 10 11 1 4 13 3,14 Figure M174-1 Cyclic behavior is broadly suggested by Blakeley and Park [1973] as described in Park & Paulay [1975]; the stress-strain response lies within the Park-Kent envelope, and is characterized by stiff initial unloading response at slope EUNL followed by a less stiff response if it unloads to less than half the current strength. Reloading stiffness degrades with increasing strain. In tension, the stress rises linearly with strain until a tensile limit FT is reached. Thereafter the stiffness and strength decays with increasing strain at a rate ESOFT. The stiffness also decays such that unloading always returns to strain at which the stress most recently changed to tensile. σult σy εsh εult Figure M174-2 MAT_RC_BEAM – reinforcement – RREINF = 4.0 6,8 3,5 9,11 12,14 15 13 7 1 10 Figure M174-3 Monotonic loading of the reinforcement results in the stress-strain curve shown, which is parabolic between εsh and εult. The same curve acts as an envelope on the hysteretic behavior, when the x-axis is cumulative plastic strain. Unloading from the yielded condition is elastic until the load reverses. Thereafter, the Bauschinger Effect (reduction in stiffness at stresses less than yield during cyclic deformation) is represented by following a Ramberg-Osgood relationship until the yield stress is reached: 𝜀 − 𝜀𝑠 = ( ) {1 + ( 𝜎𝐶𝐻 𝑟−1 ) } where 𝜀 and 𝜎 are strain and stress, 𝜀𝑠 and r and 𝜎𝐶𝐻 are as defined below is the strain at zero stress, E is Young’s Modulus, Two options are given for calculation r and 𝜎𝐶𝐻, which is performed at each stress reversal: 1. 2. If RREINF is input as -1, r and σCH are calculated internally from formulae given in Kent and Park. Parameter r depends on the number of stress reversals. Parameter 𝜎𝐶𝐻 depends on the plastic strain that occurred between the previ- ous two stress reversals. The formulae were statistically derived from experi- ments, but may not fit all circumstances. In particular, large differences in behavior may be caused by the presence or absence of small stress reversals such as could be caused by high frequency oscillations. Therefore, results might sometimes be unduly sensitive to small changes in the input data. If RREINF is entered by the user or left blank, r is held constant while 𝜎𝐶𝐻 is calculated on each reversal such that the Ramberg-Osgood curve meets the monotonic stress-strain curve at the point from which it last unloaded, e.g. points 6 and 8 are coincident in the graph below. The default setting RREINF = 4.0 gives similar hysteresis behavior to that described by Kent & Park but is unlikely to be so sensitive to small changes of input data. Output: It is recommended to use BEAMIP on *DATABASE_EXTENT_BINARY to request stress and strain output at the individual integration points. If this is done, for MAT_RC_- BEAM only, element curvature is written to the output files in place of plastic strain. In the post-processor, select “plastic strain” to display curvature (whichever of the curvatures about local y and z axes has greatest absolute value will be plotted). Alternatively, select “axial strain” to display the total axial strain (elastic + plastic) at that integration point; this can be combined with axial stress to create hysteresis plots such as those shown above. *MAT_VISCOELASTIC_THERMAL This is Material Type 175. This material model provides a general viscoelastic Maxwell model having up to 12 terms in the prony series expansion and is useful for modeling dense continuum rubbers and solid explosives. Either the coefficients of the prony series expansion or a relaxation curve may be specified to define the viscoelastic deviatoric and bulk behavior. Note that *MAT_GENERAL_VISCOELASTIC (Material Type 76) has all the capability of *MAT_VISCOELASTIC_THERMAL, and additionally offers more terms (18) in the prony series expansion and an optional scaling of material properties with moisture content. Card 1 1 Variable MID 2 RO 3 4 BULK PCF Type A8 F F F 5 EF F 6 TREF F 7 A F 8 B F If fitting is done from a relaxation curve, specify fitting parameters on card 2, otherwise if constants are set on Viscoelastic Constant Cards LEAVE THIS CARD BLANK. Card 2 1 2 3 4 5 6 7 8 Variable LCID NT BSTART TRAMP LCIDK NTK BSTARTK TRAMPK Type F I F F F I F F Viscoelastic Constant Cards. Up to 6 cards may be input. A keyword card (with a “*” in column 1) terminates this input if less than 6 cards are used. These cards are not needed if relaxation data is defined. The number of terms for the shear behavior may differ from that for the bulk behavior: simply insert zero if a term is not included. If an elastic layer is defined you only need to define GI and KI (note in an elastic layer only one card is needed). Optional Variable Type 1 Gi F 2 BETAi F 3 Ki F 4 5 6 7 8 BETAKi VARIABLE MID DESCRIPTION Material identification. A unique number or label not exceeding 8 characters must be specified. RO Mass density. BULK Elastic bulk modulus. PCF Tensile pressure elimination flag for solid elements only. If set to unity tensile pressures are set to zero. EF Elastic flag: EQ.0: the later is viscoelastic EQ.1: the layer is elastic TREF A B LCID NT Reference temperature for shift function (must be greater than zero). Coefficient for the Arrhenius and the Williams-Landel-Ferry shift functions. Coefficient for the Williams-Landel-Ferry shift function. Load curve ID for deviatoric behavior if constants, 𝐺𝑖, and 𝛽𝑖 are determined via a least squares fit. This relaxation curve is shown below. Number of terms in shear fit. If zero the default is 6. Fewer than NT terms will be used if the fit produces one or more negative shear moduli. Currently, the maximum number is set to 6. BSTART In the fit, 𝛽1 is set to zero, 𝛽2 is set to BSTART, 𝛽3 is 10 times 𝛽2, 𝛽4 is 10 times 𝛽3 , and so on. If zero, BSTART is determined by an iterative trial and error scheme. TRAMP Optional ramp time for loading. LCIDK Load curve ID for bulk behavior if constants, 𝐾𝑖, and 𝛽𝜅𝑖 are determined via a least squares fit. This relaxation curve is shown below. NTK Number of terms desired in bulk fit. If zero the default is 6. Currently, the maximum number is set to 6. BSTARTK *MAT_VISCOELASTIC_THERMAL DESCRIPTION In the fit, 𝛽𝜅1 is set to zero, 𝛽𝜅2 is set to BSTARTK, 𝛽𝜅3 is 10 times 𝛽𝜅2, 𝛽𝜅4 is 10 times 𝛽𝜅3 , and so on. If zero, BSTARTK is determined by an iterative trial and error scheme. TRAMPK Optional ramp time for bulk loading. Gi Optional shear relaxation modulus for the ith term BETAi Optional shear decay constant for the ith term Ki Optional bulk relaxation modulus for the ith term BETAKi Optional bulk decay constant for the ith term σ∕ε TRAMP 10n 10n+1 10n+2 10n+3 time optional ramp time for loading Figure M175-1. Relaxation curve. This curve defines stress versus time where time is defined on a logarithmic scale. For best results, the points defined in the load curve should be equally spaced on the logarithmic scale. Furthermore, Furthermore, the load curve should be smooth and defined in the positive quadrant. If nonphysical values are determined by least squares fit, LS-DYNA will terminate with an error message after the initialization phase is completed. If the ramp time for loading is included, then the relaxation which occurs during the loading phase is taken into account. This effect may or may not be important Remarks: Rate effects are taken into accounted through linear viscoelasticity by a convolution integral of the form: 𝜎𝑖𝑗 = ∫ 𝑔𝑖𝑗𝑘𝑙(𝑡 − 𝜏) ∂𝜀𝑘𝑙 ∂𝜏 𝑑𝜏 where 𝑔𝑖𝑗𝑘𝑙(𝑡−𝜏) is the relaxation functions for the different stress measures. This stress is added to the stress tensor determined from the strain energy functional. If we wish to include only simple rate effects, the relaxation function is represented by six terms from the Prony series: 𝑔(𝑡) = ∑ 𝐺𝑚𝑒−𝛽𝑚𝑡 𝑚=1 We characterize this in the input by shear moduli, 𝐺𝑖, and decay constants, 𝛽𝑖. An arbitrary number of terms, up to 6, may be used when applying the viscoelastic model. For volumetric relaxation, the relaxation function is also represented by the Prony series in terms of bulk moduli: 𝑘(𝑡) = ∑ 𝐾𝑚𝑒−𝛽𝑘𝑚𝑡 𝑚=1 The Arrhenius and Williams-Landel-Ferry (WLF) shift functions account for the effects of the temperature on the stress relaxation. A scaled time, t’, 𝑡′ = ∫ Φ(𝑇)𝑑𝑡 is used in the relaxation function instead of the physical time. The Arrhenius shift function is Φ(𝑇) = exp [−𝐴 ( − 𝑇REF )] and the Williams-Landel-Ferry shift function is Φ(𝑇) = exp (−𝐴 𝑇 − 𝑇REF 𝐵 + 𝑇 − 𝑇REF ) If all three values (TREF, A, and B) are not zero, the WLF function is used; the Arrhenius function is used if B is zero; and no scaling is applied if all three values are zero. . *MAT_QUASILINEAR_VISCOELASTIC Purpose: This is Material Type 176. This is a quasi-linear, isotropic, viscoelastic material based on a one-dimensional model by Fung [1993], which represents biological soft tissues such as brain, skin, kidney, spleen, etc. This model is implemented for solid and shell elements. The formulation has recently been changed to allow larger strains, and, in general, will not give the same results as the previous implementation which remains the default. Card 1 1 Variable MID 2 RO Type A8 F 3 K F Default none none none Card 2 1 2 3 4 5 LC1 LC2 I 0 4 I 0 5 Variable SO E_MIN E_MAX GAMA1 GAMA2 Type F F F F F 6 N F 6 6 K F 7 GSTART F 1/TMAX 7 EH F Default 0.0 -0.9 5.1 0.0 0.0 0.0 0.0 Viscoelastic Constant Card 1. Additional Card for LC1 = 0. Card 3 Variable 1 G1 2 BETA1 Type F F 3 G2 F 4 BETA2 F 5 G3 F 6 BETA3 F 7 G4 F 8 M F 6 8 FORM I 0 8 BETA4 Viscoelastic Constant Card 2. Additional Card for LC1 = 0. Card 4 Variable 1 G5 2 BETA5 Type F F 3 G6 F 4 BETA6 F 5 G7 F 6 BETA7 F 7 G8 F 8 BETA8 F Viscoelastic Constant Card 3. Additional Card for LC1 = 0. Card 5 Variable 1 G9 2 3 4 5 6 7 8 BETA9 G10 BETA10 G11 BETA11 G12 BETA12 Type F F F F F F F F Instantaneous Elastic Reponses Card. Additional Card for LC2 = 0. Card Variable 1 C1 Type F 2 C2 F 3 C3 F 4 C4 F 5 C5 F 6 C6 F 7 8 VARIABLE DESCRIPTION MID RO K LC1 Material identification. A unique number or label not exceeding 8 characters must be specified. Mass density. Bulk modulus. Load curve ID that defines the relaxation function in shear. This curve is used to fit the coefficients Gi and BETAi. If zero, define the coefficients directly. The latter is recommended. VARIABLE LC2 N DESCRIPTION Load curve ID that defines the instantaneous elastic response in compression and tension. If zero, define the coefficients directly. Symmetry is not assumed if only the tension side is define; therefore, defining the response in tension only, may lead to nonphysical behavior in compression. Also, this curve should give a softening response for increasing strain without any negative or zero slopes. A stiffening curve or one with negative slopes is generally unstable. Number of terms used in the Prony series, a number less than or equal to 6. This number should be equal to the number of decades of time covered by the experimental data. Define this number if LC1 is nonzero. Carefully check the fit in the d3hsp file to ensure that it is valid, since the least square fit is not always reliable. GSTART Starting value for least square fit. If zero, a default value is set equal to the inverse of the largest time in the experiment. Define this number if LC1 is nonzero. M SO Number of terms used to determine the instantaneous elastic response. This variable is ignored with the new formulation but is kept for compatibility with the previous input. Strain (logarithmic) output option to control what is written as component 7 to the d3plot database. (LS-PrePost always blindly labels this component as effective plastic strain.) The maximum values are updated for each element each time step: EQ.0.0: maximum principal strain that occurs during the calculation, EQ.1.0: maximum magnitude of the principal strain values that occurs during the calculation, EQ.2.0: maximum effective strain that occurs during the calculation. E_MIN Minimum strain used to generate the load curve from 𝐶𝑖. The default range is -0.9 to 5.1. The computed solution will be more accurate if the user specifies the range used to fit the 𝐶𝑖. Linear extrapolation is used outside the specified range. E_MAX Maximum strain used to generate the load curve from 𝐶𝑖. *MAT_QUASILINEAR_VISCOELASTIC DESCRIPTION K Material failure parameter that controls the volume enclosed by the failure surface, see *MAT_SIMPLIFIED_RUBBER. LE.0.0: ignore failure criterion; GT.0.0: use actual K value for failure criterions. GAMA1 Material failure parameter, see *MAT_SIMPLIFIED_RUBBER and Figure M181-1. GAMA2 Material failure parameter, see *MAT_SIMPLIFIED_RUBBER. EH Damage parameter, see *MAT_SIMPLIFIED_RUBBER. FORM Gi BETAi Formulation of model. FORM = 0 gives the original model developed by Fung, which always relaxes to a zero stress state as time approaches infinity, and FORM = 1 gives the alternative model, which relaxes to the quasi-static elastic response. In general, the two formulations won’t give the same responses. Formulation, FORM = -1, is an improvement on FORM = 0 where the instantaneous elastic response is used in the viscoelastic stress update, not just in the relaxation, as in FORM = 0. Consequently, the constants for the elastic response do not need to be scaled. Coefficients of the relaxation function. The number of coefficients is currently limited to 6 although 12 may be read in to maintain compatibility with the previous formulation’s input. Define these coefficients if LC1 is set to zero. At least 2 coefficients must be nonzero. Decay constants of the relaxation function. Define these coefficients if LC1 is set to zero. The number of coefficients is currently limited to 6 although 12 may be read in to maintain compatibility with the previous formulation’s input. Ci Coefficients of the instantaneous elastic response in compression and tension. Define these coefficients only if LC2 is set to zero. Remarks: The equations for the original model (FORM = 0) are given as: 𝜎𝑉(𝑡) = ∫ 𝐺(𝑡 − 𝜏) ∂𝜎𝜀[𝜀(𝜏)] ∂𝜀 ∂𝜀 ∂𝜏 𝑑𝜏 𝐺(𝑡) = ∑ 𝐺𝑖 𝑒−𝛽𝑡 𝑖=1 𝜎𝜀(𝜀) = ∑ 𝐶𝑖 𝜀𝑖 𝑖=1 where G is the shear modulus. Effective strain (which can be written to the d3plot database) is calculated as follows: 𝜀effective = √ 𝜀𝑖𝑗𝜀𝑖𝑗 The polynomial for instantaneous elastic response should contain only odd terms if symmetric tension-compression response is desired. The new model (FORM = 1) is based on the hyperelastic model used *MAT_SIMPLI- FIED_RUBBER assuming incompressibility. The one-dimensional expression for 𝜎𝜀generates the uniaxial stress-strain curve and an additional visco-elastic term is added on, 𝜎(𝜀, 𝑡) = 𝜎𝑆𝑅(𝜀) + 𝜎𝑉(𝑡) 𝜎𝑉(𝑡) = ∫ 𝐺(𝑡 − 𝜏) ∂𝜀 ∂𝜏 𝑑𝜏 where the first term to the right of the equals sign is the hyperelastic stress and the second is the viscoelastic stress. Unlike the previous formulation, where the stress always relaxed to zero, the current formulation relaxes to the hyperelastic stress. *MAT_HILL_FOAM Purpose: This is Material Type 177. This is a highly compressible foam based on the strain-energy function proposed by Hill [1979]; also see Storakers [1986]. Poisson’s ratio effects are taken into account. 5 6 7 8 MU LCID FITTYPE LCSR Card 1 1 Variable MID 2 RO Type A8 F 3 K F Default none none none 4 N F 0 F 0 Material Constant Card 1. Additional card for LCID = 0. Card 2 Variable 1 C1 Type F 2 C2 F 3 C3 F 4 C4 F 5 C5 F Material Constant Card 2. Additional card for LCID = 0. 3 B3 F 3 4 B4 F 4 5 B5 F 5 Card 3 Variable 1 B1 Type F Card 4 Variable Type 1 R F 2 B2 F 2 M F I 0 6 C6 F 6 B6 F 6 I 0 7 C7 F 7 B7 F 7 I 0 8 C8 F 8 B8 F VARIABLE DESCRIPTION MID RO K N MU LCID Material identification. A unique number or label not exceeding 8 characters must be specified. Mass density. Bulk modulus. This modulus is used for determining the contact interface stiffness. Material constant. Define if LCID = 0 below; otherwise, N is fit from the load curve data. See equations below. Damping coefficient. Load curve ID that defines the force per unit area versus the stretch ratio. This curve can be given for either uniaxial or biaxial data depending on FITTYPE. FITTYPE Type of fit: EQ.1: uniaxial data, EQ.2: biaxial data, EQ.3: pure shear data. LCSR Load curve ID that defines the uniaxial or biaxial stretch ratio versus the transverse stretch ratio. Material constants. See equations below. Define up to 8 coefficients if LCID = 0. Material constants. See equations below. Define up to 8 coefficients if LCID = 0. Mullins effect model r coefficient Mullins effect model m coefficient Ci Bi R M Remarks: If load curve data is defined, the fit generated by LS-DYNA must be closely checked in the D3HSP output file. It may occur that the nonlinear least squares procedure in LS- DYNA, which is used to fit the data, is inadequate. The Hill strain energy density function for this highly compressible foam is given by: 𝑊 = ∑ 𝑗=1 𝐶𝑗 𝑏𝑗 𝑏𝑗 + 𝜆2 𝑏𝑗 + 𝜆3 [𝜆1 𝑏𝑗 − 3 + (𝐽−𝑛𝑏𝑗 − 1)] where 𝐶𝑗, 𝑏𝑗, and n are material constants and 𝐽 = 𝜆1𝜆2𝜆3 represents the ratio of the deformed to the undeformed state. The constant m is internally set to 4. In case number of points in the curve is less than 8, then m is set to the number of points divided by 2. The principal Cauchy stresses are 𝑡𝑖 = ∑ 𝑗=1 𝐶𝑗 𝑏𝑗 − 𝐽−𝑛𝑏𝑗] 𝑖 = 1,2,3 [𝜆𝑖 From the above equations the shear modulus is: and the bulk modulus is: 𝜇 = ∑ 𝐶𝑗𝑏𝑗 𝑗=1 𝐾 = 2𝜇 (𝑛 + ) The value for K defined in the input is used in the calculation of contact forces and for the material time step. Generally, this value should be equal to or greater that the K given in the above equation. *MAT_VISCOELASTIC_HILL_FOAM Purpose: This is Material Type 178. This is a highly compressible foam based on the strain-energy function proposed by Hill [1979]; also see Storakers [1986]. The extension to include large strain viscoelasticity is due to Feng and Hallquist [2002]. 5 6 7 8 MU LCID FITTYPE LCSR 4 N F 0 4 Card 1 1 Variable MID 2 RO Type A8 F 3 K F Default none none none Card 2 1 2 3 Variable LCVE NT GSTART Type Default I 0 F 6 F 1/TMAX F 0.05 5 Material Constant Card 1. Additional card for LCID = 0. Card 3 Variable 1 C1 Type F 2 C2 F 3 C3 F 4 C4 F 5 C5 F Material Constant Card 2. Additional card for LCID = 0. Card 4 Variable 1 B1 Type F 2 B2 F 3 B3 F 4 B4 F 5 B5 F I 0 6 6 C6 F 6 B6 F I 0 7 7 C7 F 7 B7 F I 0 8 8 C8 F 8 B8 Viscoelastic Constant Cards. Up to 12 cards may be input. A keyword card (with a “*” in column 1) terminates this input if less than 12 cards are used. Card 5 Variable Type 1 GI F 2 3 4 5 6 7 8 BETAI F VARIABLE DESCRIPTION MID RO K N MU LCID Material identification. A unique number or label not exceeding 8 characters must be specified. Mass density. Bulk modulus. This modulus is used for determining the contact interface stiffness. Material constant. Define if LCID = 0 below; otherwise, N is fit from the load curve data. See equations below. Damping coefficient (0.05 < recommended value < 0.50; default is 0.05). Load curve ID that defines the force per unit area versus the stretch ratio. This curve can be given for either uniaxial or biaxial data depending on FITTYPE. Load curve LCSR below must also be defined. FITTYPE Type of fit: EQ.1: uniaxial data, EQ.2: biaxial data. LCSR LCVE Load curve ID that defines the uniaxial or biaxial stress ratio versus the transverse stretch ratio. Optional load curve ID that defines the relaxation function in shear. This curve is used to fit the coefficients Gi and BETAi. If zero, define the coefficients directly. The latter is recommended. VARIABLE NT DESCRIPTION Number of terms used to fit the Prony series, which is a number less than or equal to 12. This number should be equal to the number of decades of time covered by the experimental data. Define this number if LCVE is nonzero. Carefully check the fit in the D3HSP file to ensure that it is valid, since the least square fit is not always reliable. GSTART Starting value for least square fit. If zero, a default value is set equal to the inverse of the largest time in the experiment. Define this number if LC1 is nonzero, Ci, Material constants. See equations below. Define up to 8 coefficients. Ci Bi GI Material constants. See equations below. Define up to 8 coefficients if LCID = 0. Material constants. See equations below. Define up to 8 coefficients if LCID = 0. Optional shear relaxation modulus for the ith term BETAI Optional decay constant if ith term Remarks: If load curve data is defined, the fit generated by LS-DYNA must be closely checked in the D3HSP output file. It may occur that the nonlinear least squares procedure in LS- DYNA, which is used to fit the data, is inadequate. The Hill strain energy density function for this highly compressible foam is given by: 𝑝𝑛+1 = 𝑝𝑛𝑒−𝛽⋅𝛥𝑡 + 𝐾𝜀̇𝑘𝑘 ( 1 − 𝑒−𝛽⋅𝛥𝑡 ) where 𝛽 = |𝐵𝐸𝑇𝐴| where 𝐶𝑗, 𝑏𝑗, and n are material constants and 𝐽 = 𝜆1𝜆2𝜆3 represents the ratio of the deformed to the undeformed state. The principal Cauchy stresses are 𝑡𝑖 = ∑ 𝑗=1 𝐶𝑗 𝑏𝑗 − 𝐽−𝑛𝑏𝑗] 𝑖 = 1,2,3 [𝜆𝑖 From the above equations the shear modulus is: 𝜇 = ∑ 𝐶𝑗𝑏𝑗 𝑗=1 and the bulk modulus is: 𝐾 = 2𝜇 (𝑛 + ) The value for K defined in the input is used in the calculation of contact forces and for the material time step. Generally, this value should be equal to or greater that the K given in the above equation. Rate effects are taken into account through linear viscoelasticity by a convolution integral of the form: 𝜎𝑖𝑗 = ∫ 𝑔𝑖𝑗𝑘𝑙 (𝑡 − 𝜏) ∂𝜀𝑘𝑙 ∂𝜏 𝑑𝜏 or in terms of the second Piola-Kirchhoff stress, 𝑆𝑖𝑗, and Green's strain tensor, 𝐸𝑖𝑗, 𝑆𝑖𝑗 = ∫ 𝐺𝑖𝑗𝑘𝑙 (𝑡 − 𝜏) ∂ 𝐸𝑘𝑙 ∂𝜏 𝑑𝜏 where 𝑔𝑖𝑗𝑘𝑙(𝑡 − 𝜏) and 𝐺𝑖𝑗𝑘𝑙(𝑡 − 𝜏) are the relaxation functions for the different stress measures. This stress is added to the stress tensor determined from the strain energy functional. If we wish to include only simple rate effects, the relaxation function is represented by six terms from the Prony series: given by, 𝑔(𝑡) = 𝛼0 + ∑ 𝛼𝑚 𝑚=1 𝑒−𝛽 𝑡 𝑔(𝑡) = ∑ 𝐺𝑖𝑒−𝛽𝑖 𝑡 𝑖=1 This model is effectively a Maxwell fluid which consists of a dampers and springs in series. We characterize this in the input by shear moduli, 𝐺𝑖, and decay constants, 𝛽𝑖. The viscoelastic behavior is optional and an arbitrary number of terms may be used. *MAT_LOW_DENSITY_SYNTHETIC_FOAM_{OPTION} This is Material Type 179 (and 180 if the ORTHO option below is active) for modeling rate independent low density foams, which have the property that the hysteresis in the loading-unloading curve is considerably reduced after the first loading cycle. In this material we assume that the loading-unloading curve is identical after the first cycle of loading is completed and that the damage is isotropic, i.e., the behavior after the first cycle of loading in the orthogonal directions also follows the second curve. The main application at this time is to model the observed behavior in the compressible synthetic foams that are used in some bumper designs. Tables may be used in place of load curves to account for strain rate effects. Available options include: <BLANK> ORTHO WITH_FAILURE ORTHO_WITH_FAILURE If the foam develops orthotropic behavior, i.e., after the first loading and unloading cycle the material in the orthogonal directions are unaffected then the ORTHO option should be used. If the ORTHO option is active the directionality of the loading is stored. This option is requires additional storage to store the history variables related to the orthogonality and is slightly more expensive. An optional failure criterion is included. A description of the failure model is provided below for material type 181, *MAT_SIMPLIFIED_RUBBER/FOAM. Card 1 1 Variable MID 2 RO Type A8 F 3 E F 4 5 LCID1 LCID2 F F Default 6 HU F 1. 7 8 BETA DAMP F F 0.05 Card 2 1 2 3 4 5 6 7 Variable SHAPE FAIL BVFLAG ED BETA1 KCON REF Type F F F F F F F 8 TC F Default 1.0 0.0 0.0 0.0 0.0 0.0 0.0 1.E+20 Additional card for LCID1 < 0. Card 3 1 2 3 4 5 6 7 8 Variable RFLAG DTRT Type F F Default 0.0 0.0 Additional card for WITH_FAILURE keyword option. Card 4 Variable Type 1 K F 2 3 GAMA1 GAMA2 F F 4 EH F 5 6 7 8 VARIABLE DESCRIPTION MID RO E Material identification. A unique number or label not exceeding 8 characters must be specified. Mass density Young’s modulus. This modulus is used if the elongations are tensile as described for the *MAT_LOW_DENSITY_FOAM. VARIABLE DESCRIPTION LCID1 Load curve or table ID: LCID2 HU BETA DAMP GT.0: Load curve ID, see *DEFINE_CURVE, for nominal stress versus strain for the undamaged material. LT.0: -LCID1 is Table ID, see *DEFINE_TABLE, for nominal stress versus strain for the undamaged material as a function of strain rate Load curve or table ID. The load curve ID, see *DEFINE_CURVE, defines the nominal stress versus strain for the damaged material. The table ID, see *DEFINE_TABLE, defines the nominal stress versus strain for the damaged material as a function of strain rate Hysteretic unloading factor between 0 and 1 (default = 1, i.e., no energy dissipation), see also Figure M179-1. β, decay constant to model creep in unloading Viscous coefficient (.05 < recommended value <.50) to model damping effects. LT.0.0: |DAMP| is the load curve ID, which defines the damping constant as a function of the maximum strain in compression defined as: 𝜀max = max(1 − 𝜆1, 1 − 𝜆2, 1. −𝜆3). In tension, the damping constant is set to the value corre- sponding to the strain at 0. The abscissa should be defined from 0 to 1. SHAPE Shape factor for unloading. Active for nonzero values of the hysteretic unloading factor. Values less than one reduces the energy dissipation and greater than one increases dissipation, see also Figure M179-1 FAIL Failure option after cutoff stress is reached: EQ.0.0: tensile stress remains at cut-off value, EQ.1.0: tensile stress is reset to zero. BVFLAG Bulk viscosity activation flag, see remark below: EQ.0.0: no bulk viscosity (recommended), EQ.1.0: bulk viscosity active. ED BETA1 KCON *MAT_LOW_DENSITY_SYNTHETIC_FOAM DESCRIPTION Optional Young's relaxation modulus, 𝐸𝑑, for rate effects. See comments below. Optional decay constant, 𝛽1. Stiffness coefficient for contact interface stiffness. If undefined the maximum slope in stress vs. strain curve is used. When the maximum slope is taken for the contact, the time step size for this material is reduced for stability. In some cases Δt may be significantly smaller, and defining a reasonable stiffness is recommended. REF Use reference geometry to initialize the stress tensor. The reference geometry is defined by the keyword:*INITIAL_FOAM_- REFERENCE_GEOMETRY . EQ.0.0: off, EQ.1.0: on. TC Tension cut-off stress RFLAG Rate type for input: EQ.0.0: LCID1 and LCID2 should be input as functions of true strain rate EQ.1.0: LCID1 and LCID2 should be input as functions of engineering strain rate. DTRT Strain rate averaging flag: EQ.0.0: use weighted running average LT.0.0: average the last 11 values GT.0.0: average over the last DTRT time units. K Material failure parameter that controls the volume enclosed by the failure surface. LE.0.0: ignore failure criterion; GT.0.0: use actual K value for failure criterions. GAMA1 Material failure parameter, see equations below and Figure M181-1. GAMA2 Material failure parameter, see equations below. Loading curve for first cycle Loading curve for second and subsequent cycles Strain Figure M179-1. Loading and reloading curves. VARIABLE DESCRIPTION EH Damage parameter. Remarks: This model is based on *MAT_LOW_DENSITY_FOAM. The uniaxial response is shown below with a large shape factor and small hysteretic factor. If the shape factor is not used, the unloading will occur on the loading curve for the second and subsequent cycles. The damage is defined as the ratio of the current volume strain to the maximum volume strain, and it is used to interpolate between the responses defined by LCID1 and LCID2. HU defines a hysteretic scale factor that is applied to the stress interpolated from LCID1 and LCID2, 𝜎 = [HU + (1 − HU) × min (1, 𝑒int max) 𝑒int ] 𝜎(LCID1,LCID2) where eint is the internal energy and S is the shape factor. Setting HU to 1 results in a scale factor of 1. Setting HU close to zero scales the stress by the ratio of the internal energy to the maximum internal energy raised to the power S, resulting in the stress being reduced when the strain is low. *MAT_SIMPLIFIED_RUBBER/FOAM_{OPTION} This is Material Type 181. This material model provides a rubber and foam model defined by a single uniaxial load curve or by a family of uniaxial curves at discrete strain rates. The definition of hysteretic unloading is optional and can be realized via a single uniaxial unloading curve or a two-parameter formulation (starting with 971 release R5). The foam formulation is triggered by defining a Poisson’s ratio. This material may be used with both shell and solid elements. Available options include: <BLANK> WITH_FAILURE LOG_LOG_INTERPOLATION When the WITH_FAILURE keyword option is active, a strain based failure surface is defined suitable for incompressible polymers modeling failure in both tension and compression. This material collaboration with Paul Du Bois, LSTC, and Prof. Dave J. Benson, UCSD. law has been developed at DaimlerChrysler, Sindelfingen, in Card 1 1 Variable MID Type A8 Card 2 1 2 RO F 2 3 KM F 3 4 MU F 4 5 G F 5 6 7 8 SIGF REF PRTEN F 6 F 7 F 8 Variable SGL SW ST LC /TBID TENSION RTYPE AVGOPT PR/BETA Type F F F F F F F Additional card required for WITH_FAILURE option. Otherwise skip this card. 5 6 7 8 Card 3 Variable Type 1 K F 2 3 GAMA1 GAMA2 F F 4 EH F Optional Parameter Card. Card 4 1 2 3 4 5 6 7 8 Variable LCUNLD HU SHAPE STOL VISCO Type F F F F F Optional Viscoelastic Constants Cards. Up to 12 card in format 5 may be input. A keyword card (with a “*” in column 1) terminates this input if less than 12 cards are used. 1 Gi F Card 5 Variable Type Default 2 3 4 5 6 7 8 BETAi VFLAG F I 0 VARIABLE DESCRIPTION MID RO KM MU Material identification. A unique number or label not exceeding 8 characters must be specified. Mass density Linear bulk modulus. Damping coefficient (0.05 < recommended value < 0.50; default is 0.10). VARIABLE DESCRIPTION G SIGF REF PRTEN SGL SW ST LC/TBID Shear modulus for frequency independent damping. Frequency independent damping is based on a spring and slider in series. The critical stress for the slider mechanism is SIGF defined below. For the best results, the value of G should be 250-1000 times greater than SIGF. Limit stress for frequency independent, frictional, damping. Use reference geometry to initialize the stress tensor. The reference geometry is defined by the keyword:*INITIAL_FOAM_- REFERENCE_GEOMETRY . EQ.0.0: off, EQ.1.0: on. The tensile Poisson’s ratio for shells (optional). If PRTEN is zero, PR/BETA will serve as the Poisson’s ratio for both tension and compression in shells. If PRTEN is nonzero, PR/BETA will serve only as the compressive Poisson’s ratio for shells. Specimen gauge length Specimen width Specimen thickness Load curve or table ID, see *DEFINE_TABLE, defining the force versus actual change in the gauge length. If SGL, SW, and ST are set to unity (1.0), then curve LC is also engineering stress versus engineering strain. If the table definition is used a family of curves are defined for discrete strain rates. The load curves should cover the complete range of expected loading, i.e., the smallest stretch ratio to the largest. TENSION Parameter that controls how the rate effects are treated. Applicable to the table definition. EQ.-1.0: rate effects are considered during tension and compression loading, but not during unloading, EQ.0.0: rate effects are considered for compressive loading only, EQ.1.0: rate effects are treated identically in tension and compression. *MAT_SIMPLIFIED_RUBBER/FOAM DESCRIPTION RTYPE Strain rate type if a table is defined: EQ.0.0: true strain rate, EQ.1.0: engineering strain rate AVGOPT Averaging option determine strain rate to reduce numerical noise. LT.0.0: |AVGOPT| is a time window/interval over which the strain rates are averaged. EQ.0.0: simple average of twelve time steps, EQ.1.0: running average of last 12 averages. PR/BETA If the value is specified between 0 and 0.5 exclusive, i.e., 0 < PR < 0.50 the number defined here is taken as Poisson’s ratio. If zero, an incompressible rubber like behavior is assumed and a default value of 0.495 is used internally. If a Poisson’s ratio of 0.0 is desired, input a small value for PR such as 0.001. When fully integrated solid elements are used and when a nonzero Poisson’s ratio is specified, a foam material is assumed and selective- reduced integration is not used due to the compressibility. This is true even if PR approaches 0.500. If any other value excluding zero is defined, then BETA is taken as the absolute value of the given number and a nearly incompressible rubber like behavior is assumed. An incrementally updated mean viscous stress develops according to the equation: 𝑝𝑛+1 = 𝑝𝑛𝑒−𝛽𝛥𝑡 + 𝐾𝑚𝜀̇𝑘𝑘 ( 1 − 𝑒−𝛽𝛥𝑡 ), where 𝛽 = |BETA| and 𝐾𝑚 = KM. The BETA parameter does not apply to highly compressible foam materials. K Material failure parameter that controls the volume enclosed by the failure surface. LE.0.0: ignore failure criterion; GT.0.0: use actual K value for failure criterions. GAMA1 Material failure parameter, see equations below and Figure 181.1. GAMA2 Material failure parameter, see equations below. VARIABLE DESCRIPTION EH Damage parameter. LCUNLD HU SHAPE Load curve, see *DEFINE_CURVE, defining the force versus actual length during unloading. The unload curve should cover exactly the same range as LC or the load curves of TBID and its end points should have identical values, i.e., the combination of LC and LCUNLD or the first curve of TBID and LCUNLD describes a complete cycle of loading and unloading. See also material *MAT_083. Hysteretic unloading factor between 0 and 1 (default = 1., i.e. no energy dissipation), see also material *MAT_083 and Figure M57-1. This option is ignored if LCUNLD is used. Shape factor for unloading. Active for nonzero values of the hysteretic unloading factor HU. Values less than one reduces the energy dissipation and greater than one increases dissipation, see also material *MAT_083 and Figure M57-1. STOL Tolerance in stability check, see remarks. VISCO Viscoelasticity formulation. EQ.0.0: purely elastic; EQ.1.0: visco-elastic formulation. Gi Optional shear relaxation modulus for the ith term BETAi Optional decay constant if ith term VFLAG Flag for the viscoelasticity formulation. This appears only on the first line defining Gi, BETAi, and VFLAG. If VFLAG = 0, the standard viscoelasticity formulation is used (the default), and if the viscoelasticity the VFLAG = 1, instantaneous elastic stress is used. formulation using 1 = λ K = 30 2 = 1 K = 20 K = 1 K = 10 Figure M181-1. Failure surface for polymer for ۂ1 = 0 and ۂ2 = 0.02. Remarks: The frequency independent damping is obtained by the having a spring and slider in series as shown in the following sketch: The general failure criterion for polymers is proposed by Feng and Hallquist as friction 𝑓 (𝐼1, 𝐼2, 𝐼3) = (𝐼1 − 3) + Γ1(𝐼1 − 3)2 + Γ2(𝐼2 − 3) = 𝐾 where 𝐾 is a material parameter which controls the size enclosed by the failure surface, and 𝐼1, 𝐼2 and 𝐼3 are the three invariants of right Cauchy-Green deformation tensor (𝐂) 2 2 + 𝜆3 2 + 𝜆2 𝐼1 = C𝑖𝑖 = 𝜆1 𝐼2 = (C𝑖𝑖C𝑗𝑗 − C𝑖𝑗C𝑖𝑗) = 𝜆1 2 𝜆2 2 + 𝜆1 2 𝜆3 2 + 𝜆2 2 2 𝜆3 𝐼3 = det(𝐂) = 𝜆1 with 𝜆𝑖 are the stretch ratios in three principal directions. 2 𝜆2 2 2 𝜆3 To avoid sudden failure and numerical difficulty, material failure, which is usually a time point, is modeled as a process of damage growth. In this case, the two threshold values are chosen as (1 - h)K and K, where h (also called EH) is a small number chosen based on experimental results reflecting the range between damage initiation and material failure. The damage is defined as function of 𝑓 : 𝐷 = ⎧ {{ ⎨ {{ ⎩ [ 1 + cos 𝜋(𝑓 − 𝐾) ] ℎ𝐾 if 𝑓 ≤ (1 − ℎ)𝐾 if (1 − ℎ)𝐾 < 𝑓 < 𝐾 if 𝑓 ≥ 𝐾 This definition indicates that damage is first-order continuous. Under this definition, the tangent stiffness matrix will be continuous. The reduced stress considering damage effect is 𝑜 𝜎𝑖𝑗 = (1 − 𝐷)𝜎𝑖𝑗 𝑜 is the undamaged stress. It is assumed that prior to final failure, material where 𝜎𝑖𝑗 damage is recoverable. Once material failure occurs, damage will become permanent. The LOG_LOG_INTERPOLATION option interpolates the strain rate effect in the table TBID using log-log interpolation. Bad choices of curves for the stress-strain response may lead to an unstable model, and there is an option to check this to a certain tolerance level, see dimensionless parameter STOL. The check is done by examining the eigenvalues of the tangent modulus at selected stretch points and a warning message is issued if an eigenvalue is less than – STOL × BULK, where BULK indicates the bulk modulus of the material. For STOL < 0 the check is disabled, otherwise it should be chosen with care, a too small value may detect instabilities that are insignificant in practice. To avoid significant instabilities it is recommended to use smooth curves, at best the curves should be continuously differentiable, in fact for the incompressible case, a sufficient condition for stability is that the stress-stretch curve 𝑆(𝜆) can be written as 𝑆(𝜆) = 𝐻(𝜆) − ⎜⎛ 1 ⎟⎞ √𝜆⎠ ⎝ 𝜆√𝜆 where 𝐻(𝜆) is a function with 𝐻(1) = 0 and 𝐻′(𝜆) > 0. Rate effects are taken into account through linear viscoelasticity by a convolution integral of the form: 𝜎𝑖𝑗 = ∫ 𝑔𝑖𝑗𝑘𝑙(𝑡 − 𝜏) ∂𝜀𝑘𝑙 ∂𝜏 𝑑𝜏 or in terms of the second Piola-Kirchhoff stress, {𝑆0 }, and Green's strain tensor, {𝑆RT}, 𝑆𝑖𝑗 = ∫ 𝐺𝑖𝑗𝑘𝑙(𝑡 − 𝜏) ∂𝐸𝑘𝑙 ∂𝜏 𝑑𝜏 where 𝑔𝑖𝑗𝑘𝑙(𝑡 − 𝜏) and 𝐺𝑖𝑗𝑘𝑙(𝑡 − 𝜏) are the relaxation functions for the different stress measures. This stress is added to the stress tensor determined from the strain energy functional. If we wish to include only simple rate effects, the relaxation function is represented by six terms from the Prony series: given by, 𝑔(𝑡) = 𝛼0 + ∑ 𝛼𝑚𝑒−𝛽𝑡 𝑚=1 𝑔(𝑡) = ∑ 𝐺𝑖𝑒−𝛽𝑖𝑡 𝑖=1 This model is effectively a Maxwell fluid which consists of a dampers and springs in series. We characterize this in the input by shear moduli, 𝐺𝑖, and decay constants, 𝛽𝑖. The viscoelastic behavior is optional and an arbitrary number of terms may be used. For VFLAG = 1, the viscoelastic term is 𝜎𝑖𝑗 = ∫ 𝑔𝑖𝑗𝑘𝑙(𝑡 − 𝜏) ∂𝜎𝑘𝑙 ∂𝜏 𝑑𝜏 𝐸 is the instantaneous stress evaluated from the internal energy functional. The where 𝜎𝑘𝑙 coefficients in the Prony series therefore correspond to normalized relaxation moduli instead of elastic moduli. The Mooney-Rivlin rubber model (model 27) is obtained by specifying n = 1. In spite of the differences in formulations with model 27, we find that the results obtained with this model are nearly identical with those of material 27 as long as large values of Poisson’s ratio are used. *MAT_SIMPLIFIED_RUBBER_WITH_DAMAGE An available options includes: LOG_LOG_INTERPOLATION This is Material Type 183. This material model provides an incompressible rubber model defined by a single uniaxial load curve for loading (or a table if rate effects are considered) and a single uniaxial load curve for unloading. This model is similar to *MAT_SIMPLIFIED_RUB-BER/FOAM This material may be used with both shell and solid elements. This material collaboration with Paul Du Bois, LSTC, and Prof. Dave J. Benson, UCSD. law has been developed at DaimlerChrysler, Sindelfingen, in Card 1 1 Variable MID Type A8 Card 2 1 2 RO F 2 3 K F 3 4 MU F 4 5 G F 5 6 7 8 SIGF F 6 7 8 Variable SGL SW ST LC / TBID TENSION RTYPE AVGOPT Type F Card 3 1 F 2 F 3 F 4 F 5 F 6 F 7 8 Variable LCUNLD REF STOL Type F F F VARIABLE MID DESCRIPTION Material identification. A unique number or label not exceeding 8 characters must be specified. RO Mass density *MAT_SIMPLIFIED_RUBBER_WITH_DAMAGE DESCRIPTION K MU G SIGF SGL SW ST LC/TBID Linear bulk modulus. Damping coefficient. Shear modulus for frequency independent damping. Frequency independent damping is based of a spring and slider in series. The critical stress for the slider mechanism is SIGF defined below. For the best results, the value of G should be 250-1000 times greater than SIGF. Limit stress for frequency independent, frictional, damping. Specimen gauge length Specimen width Specimen thickness Load curve or table ID, see *DEFINE_TABLE, defining the force versus actual change in the gauge length. If SGL, SW, and ST are set to unity (1.0), then curve LC is also engineering stress versus engineering strain. If the table definition is used a family of curves are defined for discrete strain rates. The load curves should cover the complete range of expected loading, i.e., the smallest stretch ratio to the largest. TENSION Parameter that controls how the rate effects are treated. Applicable to the table definition. EQ.-1.0: rate effects are considered during tension and compression loading, but not during unloading, EQ.0.0: rate effects are considered for compressive loading only, EQ.1.0: rate effects are treated identically in tension and compression. RTYPE Strain rate type if a table is defined: EQ.0.0: true strain rate, EQ.1.0: engineering strain rate VARIABLE AVGOPT LCUNLD DESCRIPTION Averaging option determine strain rate to reduce numerical noise. EQ.0.0: simple average of twelve time steps, EQ.1.0: running 12 point average. Load curve, see *DEFINE_CURVE, defining the force versus actual change in the gauge length during unloading. The unload curve should cover exactly the same range as LC (or as the first curve of table TBID) and its end points should have identical values, i.e., the combination of LC (or as the first curve of table TBID) and LCUNLD describes a complete cycle of loading and unloading. REF Use reference geometry to initialize the stress tensor. The reference geometry is defined by the keyword:*INITIAL_FOAM_- REFERENCE_GEOMETRY . EQ.0.0: off, EQ.1.0: on. STOL Tolerance in stability check, see remark 2. Remarks: 1. The LOG_LOG_INTERPOLATION option interpolates the strain rate effect in the table TBID using log-log interpolation. 2. Bad choice of curves for the stress-strain response may lead to an unstable model, and there is an option to check this to a certain tolerance level, see di- mensionless parameter STOL. The check is done by examining the eigenvalues of the tangent modulus at selected stretch points and a warning message is issued if an eigenvalue is less than –STOL × BULK, where BULK indicates the bulk modulus of the material. For STOL < 0 the check is disabled, otherwise it should be chosen with care, a too small value may detect instabilities that are insignificant in practice. To avoid significant instabilities it is recommended to use smooth curves, at best the curves should be continuously differentiable, in fact for the incompressible case, a sufficient condition for stability is that the stress-stretch curve 𝑆(𝜆) can be written as 𝑆(𝜆) = 𝐻(𝜆) − ) 𝐻( 1 √𝜆 𝜆√𝜆 where 𝐻(𝜆) is a function with 𝐻(1) = 0 and 𝐻′(𝜆) > 0. *MAT_184 This is Material Type 184. It is a simple cohesive elastic model for use with cohesive element fomulations; see the variable ELFORM in *SECTION_SOLID and *SECTION_ SHELL. Card 1 1 2 3 4 Variable MID RO ROFLG INTFAIL Type A8 F F F 5 ET F 6 7 8 EN FN_FAIL FT_FAIL F F F VARIABLE MID DESCRIPTION Material identification. A unique number or label not exceeding 8 characters must be specified. RO Mass density ROFLG INTFAIL ET EN Flag for whether density is specified per unit area or volume. ROFLG = 0 specified density per unit volume (default), and ROFLG = 1 specifies the density is per unit area for controlling the mass of cohesive elements with an initial volume of zero. The number of integration points required for the cohesive element to be deleted. If it is zero, the element won’t be deleted even if it satisfies the failure criterion. The value of INTFAIL may range from 1 to 4, with 1 the recommended value. The stiffness in the plane of the cohesive element. The stiffness normal to the plane of the cohesive element. FN_FAIL The traction in the normal direction for tensile failure. FT_FAIL The traction in the tangential direction for shear failure. Remarks: This material cohesive model outputs three tractions having units of force per unit area into the d3plot database rather than the usual six stress components. The in plane shear traction along the 1-2 edge replaces the 𝑥-stress, the orthogonal in plane shear traction replaces the 𝑦-stress, and the traction in the normal direction replaces the 𝑧-stress. *MAT_COHESIVE_TH This is Material Type 185. It is a cohesive model by Tvergaard and Hutchinson [1992] in for use with cohesive element *SECTION_SOLID and *SECTION_SHELL. The implementation is based on the description of the implementation in the Sandia National Laboratory code, Tahoe [2003]. the variable ELFORM fomulations; see Card 1 1 2 3 4 5 6 7 8 Variable MID RO ROFLG INTFAIL SIGMAX NLS TLS Type A8 Card 2 1 F 2 F 3 F 4 F 5 F 6 F 7 8 Variable LAMDA1 LAMDA2 LAMDAF STFSF Type F F F F VARIABLE MID DESCRIPTION Material identification. A unique number or label not exceeding 8 characters must be specified. RO Mass density ROFLG INTFAIL Flag for whether density is specified per unit area or volume. ROFLG = 0 specified density per unit volume (default), and ROFLG = 1 specifies the density is per unit area for controlling the mass of cohesive elements with an initial volume of zero. The number of integration points required for the cohesive element to be deleted. If it is zero, the element won’t be deleted even if it satisfies the failure criterion. The value of INTFAIL may range from 1 to 4, with 1 the recommended value. SIGMAX Peak traction. NLS TLS 2-974 (EOS) Length scale (maximum separation) in the normal direction. ( ) t λ max reversible loading/unloadin g λ λ / fail 3 2 Λ Λ 1/ fail Λ Λ 2/ fail Figure M185-1. Relative displacement and trilinear traction-separation law VARIABLE DESCRIPTION LAMDA1 Scaled distance to peak traction (Λ1). LAMDA2 Scaled distance to beginning of softening (Λ2). LAMDAF Scaled distance for failure (Λfail). STFSF Penetration stiffness multiplier. The penetration stiffness, PS, in terms of input parameters becomes: PS = STFSF × SIGMAX NLS × (LAMDA1 LAMDAF ) Remarks: In this cohesive material model, a dimensionless separation measure λ is used, which grasps for the interaction between relative displacements in normal (δ3 - mode I) and tangential (δ1, δ2 - mode II) directions : 𝜆 = √( 𝛿1 TLS ) + ( 𝛿2 TLS ) + ( ) ⟨𝛿3⟩ NLS where the Mc-Cauley bracket is used to distinguish between tension (δ3≥0) and compression (δ3 < 0). NLS and TLS are critical values, representing the maximum separations in the interface in normal and tangential direction. For stress calculation, a trilinear traction-separation law is used, which is given by : 𝑡(𝜆) = 𝜎max ⎧ { { { ⎨ { { { ⎩ 𝜎max 𝜎max Λ1/Λfail 1 − 𝜆 1 − Λ2/Λfail 𝜆 < Λ1/Λfail Λ1/Λfail < 𝜆 < Λ2/Λfail Λ2/Λfail < 𝜆 < 1 With these definitions, the traction drops to zero when 𝜆 = 1. Then, a potential 𝜙 is defined as: 𝜙(𝛿1, 𝛿2, 𝛿3) = NLS × ∫ 𝑡(𝜆̅̅̅̅) 𝑑𝜆̅̅̅̅ Finally, tangential components (t1, t2) and normal component (t3) of the traction acting on the interface in the fracture process zone are given by: 𝑡1,2 = ∂𝜙 ∂𝛿1,2 = 𝑡(𝜆) 𝛿1,2 TLS NLS TLS , 𝑡3 = ∂𝜙 ∂𝛿3 = 𝑡(𝜆) 𝛿3 NLS which in matrix notation is NLS TLS2 ⎤ ⎥ ⎥ ⎥ ⎥ ⎥ ⎥ NLS⎦ In case of compression (𝛿3 < 0), penetration is avoided by: 𝑡1 ⎤ = ⎡ 𝑡2 ⎥ ⎢ 𝑡3⎦ ⎣ NLS TLS2 𝑡(𝜆) ⎡ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎣ 𝛿1 ⎤ ⎡ 𝛿2 ⎥ ⎢ 𝛿3⎦ ⎣ 𝑡3 = STFSF × 𝜎max NLS × Λ1/Λfail 𝛿3 Loading and unloading follows the same path, i.e. this model is completely reversible. This cohesive material model outputs three tractions having units of force per unit area into the D3PLOT database rather than the usual six stress components. The in plane shear traction t1 along the 1-2 edge replaces the x-stress, the orthogonal in plane shear traction t2 replaces the y-stress, and the traction in the normal direction t3 replaces the z- stress. *MAT_186 includes three general This is Material Type 186 and can be used only with cohesive element fomulations; see the variable ELFORM in *SECTION_SOLID and *SECTION_SHELL. The material model interaction cohesive formulations with arbitrary normalized traction-separation law given by a load curve (TSLC). These three formulations are differentiated via the type of effective separation parameter (TES). The interaction between fracture modes I and II is considered, and irreversible conditions are enforced via a damage formulation (unloading/reloading path pointing to/from the origin). See remarks for details. irreversible mixed-mode Card 1 1 2 3 4 5 6 7 8 Variable MID RO ROFLG INTFAIL TES TSLC GIC GIIC Type A8 Card 2 1 Variable XMU Type F VARIABLE MID F 2 T F F 3 S F F 4 F 5 F 6 F 7 F 8 STFSF TSLC2 F F DESCRIPTION Material identification. A unique number or label not exceeding 8 characters must be specified. RO Mass density. ROFLG INTFAIL Flag for whether density is specified per unit area or volume. ROFLG = 0 specifies density per unit volume (default), and ROFLG = 1 specifies the density is per unit area for controlling the mass of cohesive elements with an initial volume of zero. Number of integration points required for a cohesive element to be deleted. If it is zero, the element will not be deleted even if it satisfies failure criterion. The value of INTFAIL may range from 1 to 4, with 1 the recommended value. ⁄ 𝑡max 1.0 *MAT_COHESIVE_GENERAL Possible shape of TSLC 𝐴TSLC 𝜆 = 𝛿F Mode I Mode II 𝑡max 𝑇 𝑆 𝛿F 𝐺C 𝐺I 𝐴TSLC𝑇 𝐺II 𝐴TSLC𝑆 C 𝐺I C 𝐺II 𝜆0 1.0 Figure M186-1. Normalized traction-separation law VARIABLE DESCRIPTION TES Type of effective separation parameter (ESP). EQ.0.0 or 1.0: a dimensional separation measure is used. For the interaction between mode I and II, a mixed- mode propagation criterion For TES = 0.0 this is a power-law, and for TES = 1.0 this is the Benzeggagh-Kenane law [1996]. See remarks below. is used. EQ.2.0: a dimensionless separation measure is used, which grasps for the interaction between mode I displacements and mode II displacements (simi- lar to MAT_185, but with damage and general traction-separation law). See remarks below. Normalized traction-separation load curve ID. The curve must be normalized in both coordinates and must contain at least three points: (0.0, 0.0), (𝜆0, 1.0), and (1.0, 0.0), which represents the origin, the peak and the complete failure, respectively . A platform can exist in the curve like the tri-linear TSLC . Fracture toughness / energy release rate 𝐺𝐼 𝑐 for mode I Fracture toughness / energy release rate 𝐺𝐼𝐼 𝑐 for mode II Exponent that appears in the power failure criterion (TES = 0.0) or (TES = 1.0). the Recommended values for XMU are between 1.0 and 2.0. Benzeggagh-Kenane criterion failure TSLC GIC GIIC XMU T Peak traction in normal direction (mode I) VARIABLE DESCRIPTION S Peak traction in tangential direction (mode II) Penetration stiffness multiplier for compression. Factor = (1.0 + STFSF) is used to scale the compressive stiffness, i.e. no scaling is done with STFSF = 0.0 (recommended). Normalized traction-separation load curve ID for Mode II. The curve must be normalized in both coordinates and must contain at least three points: (0.0, 0.0), (𝜆0, 1.0), and (1.0, 0.0), which represents the origin, the peak and the complete failure, respectively . If not specified, TSLC is used for Mode II behavior as well. STFSF TSLC2 Remarks: All three formulations have in common that the traction-separation behavior of this 𝑐 and S for tangential mode II 𝑐 and T for normal mode I, 𝐺𝐼𝐼 model is mainly given by 𝐺𝐼 and an arbitrary normalized traction-separation load curve for both modes . The maximum (or failure) separations are then given by: 𝐹 = 𝛿𝐼 𝐺𝐼 𝐴TSLC × T , 𝛿𝐼𝐼 𝐹 = 𝐺𝐼𝐼 𝐴TSLC × S where 𝐴𝑇𝑆𝐿𝐶 is the area under the normalized traction-separation curve given with TSLC. If TSLC2 is defined 𝐹 = 𝛿𝐼 𝐺𝐼 𝐴TSLC × T , 𝛿𝐼𝐼 𝐹 = 𝐺𝐼𝐼 𝐴TSLC2 × S Where 𝐴𝑇𝑆𝐿𝐶2 is the area under the normalized traction-separation curve given with TSLC2. traction 3 2 1 Fδ II II Figure M186-2. Mixed mode traction-separation law First and second formulation (TES = 0.0 and TES = 1.0): For mixed-mode behavior, three different formulations are possible (where default TES = 0.0 with XMU = 1.0 is recommended as a first try). Here, the total mixed-mode 2 , where 𝛿𝐼 = 𝛿3 is the separation in 2 + 𝛿𝐼𝐼 relative displacement 𝛿𝑚 is defined as 𝛿𝑚 = √𝛿𝐼 2 is the separation in tangential direction 2 + 𝛿2 normal direction (mode I) and 𝛿𝐼𝐼 = √𝛿1 (mode II). See Figure M186-2. The ultimate mixed-mode displacement 𝛿𝐹 (total failure) for the power law (TES = 0.0) is: 𝛿𝐹 = 1 + 𝛽2 ⎡( ⎢ 𝐴TSLC ⎣ 𝑐) 𝐺𝐼 XMU + ( S × 𝛽2 𝐺𝐼𝐼 𝑐 ) XMU XMU − 1 ⎤ ⎥ ⎦ If TSLC2 is defined this changes to: 𝛿𝐹 = 1 + 𝛽2 𝐴TSLC × T 𝐺𝐼 ⎡( ⎢ ⎣ XMU ) + ( 𝐴TSLC2 × S × 𝛽2 𝐺𝐼𝐼 ) XMU XMU − 1 ⎤ ⎥ ⎦ and alternatively for the Benzeggagh-Kenane law [1996] (TES = 1.0): 𝛿𝐹 = 1 + 𝛽2 ⎡𝐺𝐼 ⎢ 𝐴TSLC(T + S × 𝛽2) ⎣ 𝑐 + (𝐺𝐼𝐼 𝑐 − 𝐺𝐼 𝑐) ( XMU S × 𝛽2 𝑇 + S × 𝛽2) ⎤ ⎥ ⎦ If TSLC2 is defined this changes to: 𝛿𝐹 = 1 + 𝛽2 𝐴TSLC × T + 𝐴TSLC2 × S × 𝛽2 𝑐 + (𝐺𝐼𝐼 𝑐 − 𝐺𝐼 𝑐) ( ⎡𝐺𝐼 ⎢ ⎣ 𝐴TSLC2 × S × 𝛽2 𝐴TSLC × 𝑇 + 𝐴TSLC2 × S × 𝛽2) XMU ⎤ ⎥ ⎦ where 𝛽 = 𝛿𝐼𝐼/𝛿𝐼 is the “mode mixity”. The larger the exponent XMU is chosen, the larger the fracture toughness in mixed-mode situations will be. In this model, damage irreversible conditions are enforced with of the interface is considered, i.e. loading/unloading paths coming from/pointing to the origin. This formulation is similar to MAT_COHESIVE_MIXED_MODE (MAT_138), but with the arbitrary traction-separation law TSLC. Third formulation (TES = 2.0): Here, a dimensionless effective separation parameter 𝜆 is used, which grasps for the interaction between relative displacements in normal (𝛿3 - mode I) and tangential (𝛿1,𝛿2 - mode II) directions: 𝜆 = √ √√ ⎷ ( 𝛿1 𝐹 ) 𝛿𝐼𝐼 + ( 𝛿2 𝐹 ) 𝛿𝐼𝐼 + ⟨ 𝛿3 𝐹⟩ 𝛿𝐼 𝐹 and 𝛿𝐼𝐼 where the Mc-Cauley bracket is used to distinguish between tension (𝛿3 ≥ 0) and 𝐹 are critical values, representing the maximum compression (𝛿3 < 0). 𝛿𝐼 separations in the interface in normal and tangential direction . For stress calculation, the normalized traction-separation load curve TSLC is used: 𝑡 = 𝑡max × 𝑡 ̅(𝜆). This formulation is similar to MAT_COHESIVE_TH (MAT_185), but with the arbitrary traction-separation law and a damage formulation (i.e. irreversible conditions are enforced with loading/unloading paths coming from/pointing to the orig *MAT_SAMP-1 Purpose: This is Material Type 187 (Semi-Analytical Model for Polymers). This material model uses an isotropic C-1 smooth yield surface for the description of non-reinforced plastics. Details of the implementation are given in [Kolling, Haufe, Feucht and Du Bois 2005]. This material collaboration with Paul Du Bois and Dynamore, Stuttgart. law has been developed at DaimlerChrysler, Sindelfingen, in Card 1 1 Variable MID Type A8 Card 2 1 2 RO F 2 3 4 5 6 7 8 BULK GMOD EMOD NUE RBCFAC NUMINT F 3 F 4 F 5 F 6 F 7 8 Variable LCID-T LCID-C LCID-S LCID-B NUEP LCID-P INCDAM Type I Card 3 1 I 2 I 3 I 4 F 5 I 6 7 8 Variable LCID-D EPFAIL DEPRPT LCID_TRI LCID_LC Type I Card 4 1 F 2 F 3 I 4 I 5 6 7 8 Variable MITER MIPS INCFAIL ICONV ASAF Type I I I I *MAT_SAMP-1 Optional Card. *MAT_187 Card 5 1 2 3 4 5 6 7 8 Variable LCEMOD BETA FILT Type F F F VARIABLE MID DESCRIPTION Material identification. A unique number or label not exceeding 8 characters must be specified. RO Mass density BULK Bulk modulus, used by LS-DYNA in the time step calculation GMOD Shear modulus, used by LS-DYNA in the time step calculation EMOD Young’s modulus NUE Poisson ratio qs t qbt linear extrapolation qc qbc rbcfac > 1 rbcfac = 1 rbcfac < 1 rbcfac = 0.5 (lower bound) von Mises stress pressure required input optional input biaxial tension bt tension t shear s compression c bc biaxial compression q p data data rbcfac = qbc qc extrapolated data Figure M187-1. von Mises stress as a function of pressure VARIABLE RBCFAC DESCRIPTION Ratio of yield in biaxial compression vs. yield in uniaxial compression. If RBCFAC is nonzero and all four curves LCID-T, LCID-C, LCID-S, and LCID-B are defined, a piecewise-linear yield surface as shown in Figure M187-1 is activated. See Remark 3. Default is 0. NUMINT Number of integration points which must fail before the element is deleted. This option is available for shells and solids. LT.0.0: |NUMINT| is percentage of integration points/layers which must fail before shell element fails. For fully in- tegrated shells, a methodology is used where a layer fails if one integration point fails and then the given percentage of layers must fail before the element fails. Only available for shells. *MAT_SAMP-1 VARIABLE LCID-T LCID-C LCID-S LCID-B NUEP LCID-P *MAT_187 DESCRIPTION Load curve or table ID giving the yield stress as a function of plastic strain, these curves should be obtained from quasi-static and (optionally) dynamic uniaxial tensile tests, this input is mandatory and the material model will not work unless at least one tensile stress-strain curve is given. If LCID-T is a table ID, the table values are plastic strain rates, and a curve of yield stress versus plastic strain must be given for each of those strain rates. If the first value in the table is negative, LS-DYNA assumes that all the table values represent the natural logarithm of plastic strain rate. When the highest plastic strain rate is several orders of magnitude greater than the lowest strain rate, it is recommended that the natural log of plastic strain rate be input in the table. See Remark 4. Load curve ID giving the yield stress as a function of plastic strain, this curve should be obtained from a quasi-static uniaxial compression test, this input is optional. Load curve ID giving the yield stress as a function of plastic strain, this curve should be obtained from a quasi-static shear test, this input is optional. Load curve ID giving the yield stress as a function of plastic strain, this curve should be obtained from a quasi-static biaxial tensile test, this input is optional. Plastic Poisson’s ratio: an estimated ratio of transversal to longitudinal plastic rate of deformation under uniaxial loading should be given. Load curve ID giving the plastic Poisson's ratio as a function of plastic strain during uniaxial tensile and uniaxial compressive testing. The plastic strain on the abscissa is negative for compression and positive for tension. It is important to cover both tension and compression. If LCID-P is given, the constant value of plastic Poisson's ratio NUEP is ignored. INCDAM Flag to control the damage evolution as a function of triaxiality. EQ.0: damage evolution is independent of the triaxialty. EQ.1: an incremental formulation is used to compute the damage. LCID-D EPFAIL DEPRPT LCID_TRI LCID_LC MITER MIPS *MAT_SAMP-1 DESCRIPTION Load curve ID giving the damage parameter as a function of equivalent plastic strain during uniaxial tensile testing. By default this option assumes that effective (i.e. undamaged) yield values are used in the load curves LCID-T, LCID-C, LCID-S and LCID-B. If LCID-D is given a negative value, true (i.e. damaged) yield stress values can be used. In this case an automatic stress- strain recalibration (ASSR) algorithm is activated. The damage value must be defined in the range 0 ≤ 𝑑 < 1. If EPFAIL and DEPRPT are given, the curve is used only until the effective plastic strain reaches EPFAIL. This parameter is the equivalent plastic strain at failure. If EPFAIL is given as a negative integer, a load curve is expected that defines EPFAIL as a function of the plastic strain rate. Default value is 105. Increment of equivalent plastic strain between failure point and rupture point. Stresses will fade out to zero between EPFAIL and EPFAIL+DEPRPT. If DEPRPT is given a negative value a curve definition is expected where DEPRPT is defined as function of the triaxiality. Load curve that specifies a factor that works multiplicatively on the value of EPFAIL depending on (i.e. pressure/sigma_vm). For a triaxiality of -1/3 a value of 1.0 should be specified. triaxiality the Load curve that specifies a factor that works multiplicatively on the value of EPFAIL depending on a characteristic element length, defined as the average length of spatial diagonals. Maximum number of iterations in the cutting plane algorithm, default is set to 400 Maximum number of iterations in the secant iteration performed to enforce plane stress (shell elements only), default set to 10 INCFAIL Flag to control the failure evolution as a function of triaxiality. EQ.0: Failure evolution is independent of the triaxiality. EQ.1: Incremental formulation is used to compute the failure value. EQ.-1: the failure model is deactivated. *MAT_SAMP-1 LCID_C = 0 ⎫ }} LCID_S = 0 ⎬ }} LCID_B = 0⎭ ⇒ ⎧𝜎𝑐 = 𝜎𝑡 {{{ ⎨ {{{ ⎩ 𝜎𝑠 = 𝜎𝑡 √3 LCID_C = 0 ⎫ }} LCID_S ≠ 0 ⎬ }} LCID_B = 0⎭ LCID_C ≠ 0 ⎫ }} LCID_S = 0 ⎬ }} LCID_B = 0⎭ ⇒ 𝜎c = √3𝜎𝑡𝜎𝑠 2𝜎𝑡 − √3𝜎𝑠 ⇒ 𝜎𝑠 = 2𝜎c𝜎𝑡 √3(𝜎𝑡 + 𝜎𝑐) LCID_C = 0 ⎫ }} LCID_S = 0 ⎬ }} LCID_B ≠ 0⎭ ⇒ ⎧𝜎𝑐 = {{ ⎨ {{ ⎩ 𝜎𝑠 = 𝜎𝑡𝜎𝑏 3𝜎𝑏 − 2𝜎𝑡 𝜎𝑡𝜎𝑏 √3(2𝜎𝑏 − 𝜎𝑡) *MAT_187 𝜎vM von Misses cylinder 𝜎vM Drucker-Prager Cone ⎫ }}} ⎬ }}} ⎭ ⎫ } } } } } } } } } } } } ⎬ } } } } } } } } } } } } ⎭ Figure M187-2. Fewer than 3 load curves VARIABLE DESCRIPTION ICONV Formulation flag: EQ.0: default EQ.1: yield surface is internally modified by increasing the shear yield until a convex yield surface is achieved. ASAF Safety factor, used only if ICONV = 1, values between 1 and 2 can improve convergence, however the shear yield will be artificially increased if this option is used, default is set to 1. LCEMOD Load curve ID defining Young’s modulus as function of effective strain rate. BETA FILT Decay constant in viscoelastic law: 𝜎̇ (𝑡) = −β ∙ 𝜎(𝑡) + 𝐸(𝜀̇(𝑡)) ∙ 𝜀̇(𝑡) Factor for strain rate filtering: 𝜀̇𝑛+1 𝑎𝑣𝑔 𝜀̇𝑛 𝑎𝑣𝑔 = (1 − FILT) ∙ 𝜀̇𝑛+1 𝑐𝑢𝑟𝑟 + FILT ∙ LCID_C ≠ 0 LCID_S ≠ 0 ⎫ }} ⎬ }} LCID_B = 0⎭ ⇒ normal SAMP-1 behavior LCID_C ≠ 0 LCID_S = 0 ⎫ }} ⎬ }} LCID_B ≠ 0⎭ ⇒ 𝜎𝑠 = √3 √ 3𝜎𝑏 2𝜎𝑐𝜎𝑡 (2𝜎𝑏 + 𝜎𝑐)(2𝜎𝑏 − 𝜎𝑡) LCID_C = 0 LCID_S ≠ 0 ⎫ }} ⎬ }} LCID_B ≠ 0⎭ ⇒ 𝜎𝑐 = 6(162𝜎𝑏 2𝜎𝑠 2 + 323𝜎𝑏 2 + 𝜎𝑏𝜎𝑠 2𝜎𝑡) 2𝜎𝑡 + 3𝜎𝑠 6𝜎𝑏𝜎𝑠 2𝜎𝑡 LCID_C ≠ 0 LCID_S ≠ 0 ⎫ }} ⎬ }} LCID_B ≠ 0⎭ ⇒ overspecified, least square ⎫ } } } } } } } } } } } } } } } } ⎬ } } } } } } } } } } } } } } } } ⎭ 𝜎vM SAMP-1 yield surface defined through load curves Figure M187-3. Three or more load curves Load curves: Material SAMP-1 uses three yield curves internally to evaluate a quadratic yield surface. *MAT_SAMP-1 accepts four different kinds of yield curves, LCID_T, LCID_C, LCID_S, and LCID_B where data from tension tests (LCID_T) is always required, but the others are optional. If fewer than three curves are defined, as indicated by setting the missing load curve IDs to 0, the remaining curves are generated internally. 1. Fewer than 3 load curves. In the case of fewer than 3 load curves, a linear yield surface in the invariant space spanned by the pressure and the von Mises stress is generated using the available data. See figure M187-2. 2. Three or more load curves. See figure M187-3. Remarks: 1. Damage. If the LCID_D is given, then a damage curve as a function of equivalent plastic strains acting on the stresses is defined as shown in Figure M187-4. 𝑑 1.0 𝑑𝑐 𝜀fail 𝜀erode 𝜀𝑝 𝑝 (cid:1526)𝜀rpt Figure M187-4. EPFAIL and DEPRPT defined the failure and fading behavior of a single element. Since the damaging curve acts on the yield values, the inelastic results are ef- fected by the damage curve. As a means to circumvent this, the load curve LCID-D may be given a negative ID. This will lead to an internal conversion of from nominal to effective stresses (ASSR). 2. Unsolvable Yield Surface Case. Since the generality of arbitrary curve inputs allows unsolvable yield surfaces, SAMP may modify curves internally. This will always lead to warning messages at the beginning of the simulation run. One modification that is not allowed are negative tangents of the last two data points of any of the yield curves. 3. RBCFAC. If RBCFAC is nonzero and curves LCID-T, LCID-C, LCID-S, and LCID-B are specified, the yield surface in 𝐼1-𝜎𝑣𝑚 -stress space is constructed such that a piecewise-linear yield surface is activated. This option can help promote convergence of the plasticity algorithm. Figure M187-1 illustrates the effect of RBCFAC on behavior in biaxial compression. 4. Dynamic Amplification Factor for Yield Stress. If LCID-T is given as a table specifying strain-rate scaling of the yield stress, then the compressive, shear and biaxial yield stresses are computed by multiplying their respective static values by dynamic amplification factor (dynamic/static ratio) of the tensile yield stress. *MAT_SAMP-1 # 2 3 4 5 6 Interpretation plastic strain in tension/compression plastic strain in shear biaxial plastic strain damage volumetric plastic strain 16 plastic strain rate in tension/compression 17 plastic strain rate in shear 18 biaxial plastic strain rate *MAT_THERMO_ELASTO_VISCOPLASTIC_CREEP This is Material Type 188. In this model, creep is described separately from plasticity using Garafalo’s steady-state hyperbolic sine creep law or Norton’s power law. Viscous effects of plastic strain rate are considered using the Cowper-Symonds model. Young’s modulus, Poisson’s ratio, thermal expansion coefficient, yield stress, material parameters of Cowper-Symonds model as well as the isotropic and kinematic hardening parameters are all assumed to be temperature dependent. Application scope includes: simulation of solder joints in electronic packaging, modeling of tube brazing process, creep age forming, etc. Card 1 1 Variable MID Type A8 Card 2 1 2 RO F 2 3 E F 3 4 PR F 4 5 6 7 8 SIGY ALPHA LCSS REFTEM F 5 F 6 F 7 F 8 Variable QR1 CR1 QR2 CR2 QX1 CX1 QX2 CX2 Type F Card 3 Variable Type 1 C F Card 4 1 F 2 P F 2 F 3 F 4 F 5 F 6 F 7 F 8 LCE LCPR LCSIGY LCQR LCQX LCALPH F 3 F 4 F 5 F 6 F 7 F 8 Variable LCC LCP LCCR LCCX CRPA CRPB CRPQ CRPM Type F F F F F F F *MAT_THERMO_ELASTO_VISCOPLASTIC_CREEP Card 5 1 2 3 4 5 6 7 8 Variable CRPLAW Type F VARIABLE DESCRIPTION MID RO E PR Material identification. A unique number or label not exceeding 8 characters must be specified. Mass density. Young’s modulus Poisson’s ratio SIGY Initial yield stress ALPHA Thermal expansion coefficient LCSS Load curve ID or Table ID. The load curve ID defines effective stress versus effective plastic strain. The table ID defines for each temperature value a load curve ID giving the stress versus effective plastic strain for that temperature. The stress versus effective plastic strain curve for the lowest value of temperature is used if the temperature falls below the minimum value. Likewise, the stress versus effective plastic strain curve for the highest value of temperature is used if the temperature exceeds the maximum value. Card 2 is ignored with this option. REFTEM Reference temperature that defines thermal expansion coefficient QR1 CR1 QR2 CR2 QX1 CX1 Isotropic hardening parameter 𝑄𝑟1 Isotropic hardening parameter 𝐶𝑟1 Isotropic hardening parameter 𝑄𝑟2 Isotropic hardening parameter 𝐶𝑟2 Kinematic hardening parameter 𝑄𝜒1 Kinematic hardening parameter 𝐶𝜒1 VARIABLE DESCRIPTION QX2 CX2 C P LCE Kinematic hardening parameter 𝑄𝜒2 Kinematic hardening parameter 𝐶𝜒2 Viscous material parameter 𝐶 Viscous material parameter 𝑃 Load curve for scaling Young's modulus as a function of temperature LCPR Load curve for scaling Poisson's ratio as a function of temperature LCSIGY LCQR LCQX LCALPH LCC LCP LCCR LCCX Load curve for scaling initial yield stress as a function of temperature Load curve for scaling the isotropic hardening parameters QR1 and QR2 or the stress given by the load curve LCSS as a function of temperature Load curve for scaling the kinematic hardening parameters QX1 and QX2 as a function of temperature Load curve for scaling the thermal expansion coefficient as a function of temperature Load curve for scaling the viscous material parameter 𝐶 as a function of temperature Load curve for scaling the viscous material parameter 𝑃 as a function of temperature Load curve for scaling the isotropic hardening parameters CR1 and CR2 as a function of temperature Load curve for scaling the kinematic hardening parameters CX1 and CX2 as a function of temperature CRPA Creep law parameter 𝐴 GT.0.0: Constant value LT.0.0: Load curve ID = (-CRPA) which defines 𝐴 as a function of temperature, 𝐴(𝑇). *MAT_THERMO_ELASTO_VISCOPLASTIC_CREEP DESCRIPTION CRPB Creep law parameter 𝐵 GT.0.0: Constant value LT.0.0: Load curve ID = (-CRPB) which defines 𝐵 as a function of temperature, 𝐵(𝑇). CRPQ Creep law parameter 𝑄 = 𝐸/𝑅 where E is the activation energy and R is the universal gas constant. GT.0.0: Constant value LT.0.0: Load curve ID = (-CRPQ) which defines 𝑄 as a function of temperature, 𝑄(𝑇). CRPM Creep law parameter m GT.0.0: Constant value LT.0.0: Load curve ID = (-CRPM) which defines m as a function of temperature, 𝑚(𝑇). CRPLAW Creep law definition : EQ.0.0: Garofalo’s hyperbolic sine law (default). EQ.1.0: Norton’s power law. Remarks: If LCSS is not given any value the uniaxial stress-strain curve has the form 𝑝 )] 𝑝 )] + 𝑄𝑟2[1 − exp(−𝐶𝑟2𝜀eff 𝑝 )] + 𝑄𝜒2[1 − exp(−𝐶𝜒2𝜀eff 𝑝 ) = 𝜎0 + 𝑄𝑟1[1 − exp(−𝐶𝑟1𝜀eff + 𝑄𝜒1[1 − exp(−𝐶𝜒1𝜀eff 𝜎(𝜀eff 𝑝 )]. Viscous effects are accounted for using the Cowper-Symonds model, which scales the yield stress with the factor: 𝜀̇eff ⎟⎞ 𝐶 ⎠ For CRPLAW = 0, the steady-state creep strain rate of Garafalo’s hyperbolic sine equation is given by ⎜⎛ ⎝ 1 + . 𝑝⁄ 𝜀̇𝑐 = 𝐴[sinh(𝐵𝜏𝑒)]𝑚exp (− ). For CRPLAW = 1, the steady-state creep strain rate is given by Norton’s power law equation: 𝜀̇𝑐 = 𝐴(𝜏𝑒)𝐵𝑡𝑚. In the above, 𝜏𝑒 is the effective elastic stress in the von Mises sense, T is the temperature and t is the time. The following is a schematic overview of the resulting stress update. The multiaxial creep strain increment is given by Δ𝜀𝑐 = Δ𝜀𝑐 3𝝉 𝑒 2𝜏𝑒 where 𝛕𝑒 is the elastic deviatoric stress tensor. Similarily the plastic and thermal strain increments are given by Δ𝜺p = Δ𝜀𝑝 3𝝉 𝑒 2𝜏𝑒 𝑇 Δ𝜺𝑇 = 𝛼𝑡+Δ𝑡(𝑇 − 𝑇ref)𝑰 − 𝜺𝑡 where α is the thermal expansion coefficient (note the definition compared to that of other materials). Adding it all together, the stress update is given by 𝝈𝑡+Δ𝑡 = 𝑪𝑡+Δ𝑡(𝜺𝑡 𝑒 + Δ𝜺 − Δ𝜺𝑝 − Δ𝜺𝑐 − Δ𝜺𝑇) The plasticity is isotropic or kinematic but with a von Mises yield criterion, the subscript in the equation above indicates the simulation time of evaluation. Internally, this stress update requires the solution of a nonlinear equation in the effective stress, the viscoelastic strain increment and potentially the plastic strain increment. *MAT_ANISOTROPIC_THERMOELASTIC This is Material Type 189. This model characterizes elastic materials whose elastic properties are temperature-dependent. Card 1 1 Variable MID Type A8 Card 2 1 2 RO F 2 3 4 5 6 7 8 TA1 TA2 TA3 TA4 TA5 TA6 F 3 F 4 F 5 F 6 F 7 F 8 Variable C11 C12 C13 C14 C15 C16 C22 C23 Type F Card 3 1 F 2 F 3 F 4 F 5 F 6 F 7 F 8 Variable C24 C25 C26 C33 C34 C35 C36 C44 Type F Card 4 1 F 2 F 3 F 4 F 5 F 6 F 7 F 8 Variable C45 C46 C55 C56 C66 TGE TREF AOPT Type F F F F F F Card 5 Variable 1 XP Type F 2 YP F 3 ZP F 4 A1 F 5 A2 F 6 A3 F F 8 F 7 MACF Card 6 Variable 1 V1 Type F 2 V2 F 3 V3 F 4 D1 F 5 D2 F 6 D3 F 7 8 BETA REF F F VARIABLE DESCRIPTION MID RO TAi CIJ TGE TREF AOPT Material identification. A unique number or label not exceeding 8 characters must be specified. Mass density. Curve IDs defining the coefficients of thermal expansion for the six components of strain tensor as function of temperature. Curve IDs defining the 6×6 symmetric constitutive matrix in material coordinate system as function of temperature. Note that 1 corresponds to the a material direction, 2 to the b material direction, and 3 to the c material direction. Curve ID defining the structural damping coefficient as function of temperature. Reference temperature for the calculation of thermal loads or the definition of thermal expansion coefficients. Material TIC/MAT_002 for a complete description.) option, axes (see MAT_ANISOTROPIC_ELAS- EQ.0.0: locally orthotropic with material axes determined by element nodes 1, 2, and 4, as with *DEFINE_COORDI- NATE_NODES. EQ.1.0: locally orthotropic with material axes determined by a point in space and the global location of the element center; this is the a-direction. EQ.2.0: globally orthotropic with material axes determined by vectors defined below, as with *DEFINE_COORDI- NATE_VECTOR. EQ.3.0: locally orthotropic material axes determined by rotating the material axes about the element normal by an angle, BETA, from a line in the plane of the element defined by the cross product of the vector v with the *MAT_ANISOTROPIC_THERMOELASTIC DESCRIPTION element normal. EQ.4.0: locally orthotropic in cylindrical coordinate system with the material axes determined by a vector v, and an originating point, P, which define the centerline ax- is. LT.0.0: the absolute value of AOPT is a coordinate system ID number (CID on *DEFINE_COORDINATE_NODES, *DEFINE_COORDINATE_SYSTEM or *DEFINE_CO- ORDINATE_VECTOR). Available in R3 version of 971 and later. XP, YP, ZP XP, YP, ZP define coordinates of point p for AOPT = 1 and 4. A1, A2, A3 a1, a2, a3 define components of vector a for AOPT = 2. MACF Material axis change flag for brick elements D1, D2, D3 d1, d2, d3 define components of vector d for AOPT = 2. V1, V2, V3 v1, v2, v3 define components of vector v for AOPT = 3 and 4. BETA REF Material angle in degrees for AOPT = 3, may be overwritten on the element card, see *ELEMENT_SOLID_ORTHO. Use initial geometry to initialize the stress tensor *MAT_FLD_3-PARAMETER_BARLAT This is Material Type 190. This model was developed by Barlat and Lian [1989] for modeling sheets with anisotropic materials under plane stress conditions. This material allows the use of the Lankford parameters for the definition of the anisotropy. This particular development is due to Barlat and Lian [1989]. It has been modified to include a failure criterion based on the Forming Limit Diagram. The curve can be input as a load curve, or calculated based on the n-value and sheet thickness. Card 1 1 Variable MID Type A8 Card 2 Variable Type 1 M F Card 3 1 Variable AOPT Type F Card 4 1 Variable Type 2 RO F 2 3 E F 3 4 PR F 4 5 HR F 5 R00 R45 R90 LCID F 4 I 5 6 P1 F 6 E0 F 6 7 P2 F 7 SPI F 7 8 ITER F 8 P3 F 8 FLDCID RN RT FLDSAFE FLDNIPF F 7 F 8 I F F 4 A1 F 5 A2 F 6 A3 F F 2 C F 2 F 3 P F Variable 1 V1 Type F *MAT_FLD_3-PARAMETER_BARLAT 2 V2 F 3 V3 F 4 D1 F 5 D2 F 6 D3 F 7 8 BETA F VARIABLE DESCRIPTION MID RO E PR HR Material identification. A unique number or label not exceeding 8 characters must be specified. Mass density Young’s modulus, 𝐸 Poisson’s ratio, 𝜈 Hardening rule: EQ.1.0: linear (default) EQ.2.0: exponential (Swift) EQ.3.0: load curve EQ.4.0: exponential (Voce) EQ.5.0: exponential (Gosh) EQ.6.0: exponential (Hocket-Sherby) P1 Material parameter: HR.EQ.1.0: Tangent modulus HR.EQ.2.0: 𝑘, strength coefficient for Swift exponential hardening HR.EQ.4.0: 𝑎, coefficient for Voce exponential hardening HR.EQ.5.0: 𝑘, strength coefficient for Gosh exponential hardening HR.EQ.6.0: 𝑎, coefficient for Hocket-Sherby exponential hardening VARIABLE DESCRIPTION P2 Material parameter: HR.EQ.1.0: Yield stress HR.EQ.2.0: 𝑛, exponent for Swift exponential hardening HR.EQ.4.0: 𝑐, coefficient for Voce exponential hardening HR.EQ.5.0: 𝑛, exponent for Gosh exponential hardening HR.EQ.6.0: 𝑐, coefficient for Hocket-Sherby exponential hardening ITER Iteration flag for speed: ITER.EQ.0.0: fully iterative ITER.EQ.1.0: fixed at three iterations Generally, ITER = 0 is recommended. However, ITER = 1 is somewhat faster and may give acceptable results in most problems. M R00 R45 R90 LCID E0 m, exponent in Barlat’s yield surface 𝑅00, Lankford parameter determined from experiments 𝑅45, Lankford parameter determined from experiments 𝑅90, Lankford parameter determined from experiments load curve ID for the load curve hardening rule Material parameter HR.EQ.2.0: 𝜀0 for determining initial yield stress for Swift exponential hardening. (Default = 0.0) HR.EQ.4.0: 𝑏, coefficient for Voce exponential hardening HR.EQ.5.0: 𝜀0 for determining initial yield stress for Gosh exponential hardening. (Default = 0.0) HR.EQ.6.0: 𝑏, coefficient for Hocket-Sherby exponential hardening *MAT_FLD_3-PARAMETER_BARLAT DESCRIPTION SPI If 𝜀0 is zero above and HR.EQ.2.0. (Default = 0.0) EQ.0.0: 𝜀0 = ⁄ (𝑛−1) ⎜⎜⎜⎛𝐸 𝑘⁄ ⎝ ⎟⎟⎟⎞ ⎠ LE.0.2: 𝜀0 = SPI GT.0.2: 𝜀0 = 𝑛⁄ ⎜⎜⎜⎛SPI ⁄ ⎝ ⎟⎟⎟⎞ ⎠ P3 Material parameter: HR.EQ.5.0: 𝑝, parameter for Gosh exponential hardening HR.EQ.6.0: 𝑛, exponent for Hocket-Sherby exponential hardening AOPT Material axes option : EQ.0.0: locally orthotropic with material axes determined by element nodes 1, 2, and 4, as with *DEFINE_COORDI- NATE_NODES, and then rotated about the shell ele- ment normal by the angle BETA. EQ.2.0: globally orthotropic with material axes determined by vectors defined below, as with *DEFINE_COORDI- NATE_VECTOR. EQ.3.0: locally orthotropic material axes determined by rotating the material axes about the element normal by an angle, BETA, from a line in the plane of the element defined by the cross product of the vector v with the element normal. LT.0.0: the absolute value of AOPT is a coordinate system ID number (CID on *DEFINE_COORDINATE_NODES, *DEFINE_COORDINATE_SYSTEM or *DEFINE_CO- ORDINATE_VECTOR). Available in R3 version of 971 and later. C P 𝐶 in Cowper-Symonds strain rate model 𝑝 in Cowper-Symonds strain rate model, 𝑝 = 0.0 for no strain rate effects VARIABLE FLDCID RN RT DESCRIPTION Load curve ID defining the Forming Limit Diagram. Minor engineering strains in percent are defined as abscissa values and Major engineering strains in percent are defined as ordinate values. The forming limit diagram is shown in Figure M39-1. In defining the curve list pairs of minor and major strains starting with the left most point and ending with the right most point, see *DEFINE_CURVE. Hardening exponent equivalent to the n-value in a power law hardening law. If the parameter FLDCID is not defined, this value in combination with the value RT can be used to calculate a forming limit curve to allow for failure. Sheet thickness used for calculating a forming limit curve. This value does not override the sheet thickness in any way. It is only used in conjunction with the parameter RN to calculate a forming limit curve if the parameter FLDCID is not defined. FLDSAFE A safety offset of the forming limit curve. This value should be input as a percentage (ex. 10 not 0.10). This safety margin will be applied to the forming limit curve defined by FLDCID or the curve calculated by RN and RT. FLDNIPF Numerical integration points failure treatment. GT.0.0: The number of element integration points that must fail before the element is deleted. By default, if one inte- gration point has strains above the forming limit curve, the element is flagged for deletion. LT.0.0: The element is deleted when all integration points within a relative distance of –FLDNIPF from the mid surface have failed (value between -1.0 and 0.0). A1, A2, A3 Components of vector 𝐚 for AOPT = 2. V1, V2, V3 Components of vector 𝐯 for AOPT = 3. D1, D2, D3 Components of vector 𝐝 for AOPT = 2. BETA Material angle in degrees for AOPT = 0 and 3, may be overridden on the element card, see *ELEMENT_SHELL_BETA. See material 36 for the theoretical basis. *MAT_FLD_3-PARAMETER_BARLAT The forming limit curve can be input directly as a curve by specifying a load curve id with the parameter FLDCID. When defining such a curve, the major and minor strains must be input as percentages. Alternatively, the parameters RN and RT can be used to calculate a forming limit curve. The use of RN and RT is not recommended for non-ferrous materials. RN and RT are ignored if a non-zero FLDCID is defined. The first history variable is the maximum strain ratio defined by: 𝜀majorworkpiece 𝜀majorfld corresponding to 𝜀minorworkpiece. A value between 0 and 1 indicates that the strains lie below the forming limit curve. Values above 1 indicate that the strains are above the forming limit curve. *MAT_191 Purpose: This is Material Type 191. This material enables lumped plasticity to be developed at the ‘node 2’ end of Belytschko-Schwer beams (resultant formulation). The plastic yield surface allows interaction between the two moments and the axial force. Card 1 1 Variable MID 2 RO Type A8 F 3 E F F F 4 5 6 7 8 PR ASFLAG FTYPE DEGRAD IFEMA Default none none none none 0.0 Card 2 1 2 3 4 5 I 1 6 I 0 7 I 0 8 Variable LCPMS SFS LCPMT SFT LCAT SFAT LCAC SFAC Type F F F F F F F F Default none 1.0 LCMPS 1.0 none 1.0 LCAT 1.0 This card 3 format is used when FTYPE = 1 (default). Card 3 1 2 3 4 Variable ALPHA BETA GAMMA DELTA Type F F F F 5 A F 6 B F 7 8 FOFFS F Default see note see note see note see note see note see note 0.0 This card 3 format is used when FTYPE = 2. Card 3 1 Variable SIGY Type F 2 D F 3 W F 4 TF F 5 TW F Default none none none none none 6 7 8 This card 3 format is used when FTYPE = 4. Card 3 1 2 3 4 5 6 7 8 Variable PHI_T PHI_C PHI_B Type F F F Default 0.8 0.85 0.9 This card 3 format is used when FTYPE = 5. Card 3 1 2 3 4 5 6 7 8 Variable ALPHA BETA GAMMA DELTA PHI_T PHI_C PHI_B Type F F F F F F F Default none none 1.4 none 1.0 1.0 1.0 FEMA limits Card 1. Additional card for IFEMA > 0. Card 4 1 2 3 4 5 6 7 8 Variable PR1 PR2 PR3 PR4 Type Default F 0 F 0 F 0 F 0 FEMA limits Card 2. Additional card for IFEMA = 2. Card 5 1 2 3 4 5 6 7 8 Variable TS1 TS2 TS3 TS4 CS1 CS2 CS3 CS4 Type Default F 0 F 0 F 0 F 0 F F F F TS1 TS2 TS3 TS4 VARIABLE DESCRIPTION MID RO E PR Material identification. A unique number or label not exceeding 8 characters must be specified. Mass density. Young’s modulus. Poisson’s ratio. ASFLAG Axial strain definition for force-strain curves, degradation and FEMA output: EQ.0.0: true (log) total strain EQ.1.0: change in length EQ.2.0: nominal total strain EQ.3.0: FEMA plastic strain ( = nominal total strain minus elastic strain) *MAT_SEISMIC_BEAM DESCRIPTION FTYPE Formulation type for interaction EQ.1: Parabolic coefficients, axial load and biaxial bending (default). EQ.2: Japanese code, axial force and major axis bending. EQ.4: AISC utilization calculation but no yielding EQ.5: AS4100 utilization calculation but no yielding DEGRADE Flag for degrading moment behavior EQ.0: Behavior as in previous versions EQ.1: Fatigue-type degrading moment-rotation behavior EQ.2: FEMA-type degrading moment-rotation behavior IFEMA Flag for input of FEMA thresholds EQ.0: No input EQ.1: Input of rotation thresholds only EQ.2: Input of rotation and axial strain thresholds LCPMS Load curve ID giving plastic moment vs. Plastic rotation at node 2 about local s-axis. See *DEFINE_CURVE. SFS Scale factor on s-moment at node 2. LCPMT Load curve ID giving plastic moment vs. Plastic rotation at node 2 about local t-axis. See *DEFINE_CURVE. SFT LCAT SFAT LCAC Scale factor on t-moment at node 2. Load curve ID giving axial tensile yield force vs. total tensile (elastic + plastic) strain or vs. elongation. See AOPT above. All values are positive. See *DEFINE_CURVE. Scale factor on axial tensile force. Load curve ID giving compressive yield force vs. total compressive (elastic + plastic) strain or vs. elongation. See AOPT above. All values are positive. See *DEFINE_CURVE. SFAC Scale factor on axial tensile force. ALPHA Parameter to define yield surface. VARIABLE DESCRIPTION BETA Parameter to define yield surface. GAMMA Parameter to define yield surface. DELTA Parameter to define yield surface. A B Parameter to define yield surface. Parameter to define yield surface. FOFFS Force offset for yield surface . SIGY Yield stress of material. D W TF TW PHI_T PHI_C PHI_B Depth of section used to calculate interaction curve. Width of section used to calculate interaction curve. Flange thickness of section used to calculate interaction curve. Web thickness used to calculate interaction curve. Factor on tensile capacity, φt Factor on compression capacity, φc Factor on bending capacity, φb PR1 - PR4 Plastic rotation thresholds 1 to 4 TS1 - TS4 Tensile axial strain thresholds 1 to 4 CS1 - CS4 Compressive axial strain thresholds 1 to 4 Remarks: Yield surface for formulation type 1 is of the form: 𝜓 = ( 𝑀𝑠 𝑀𝑦𝑠 ) + ( 𝑀𝑡 𝑀𝑦𝑡 ) + 𝐴 ( 𝐹𝑦 ) + 𝐵 ( ) − 1 𝐹𝑦 Where, 𝑀𝑠, 𝑀𝑡 = moments about local s and t axes 𝑀𝑦𝑠, 𝑀𝑦𝑡 = current yield moments 𝐹 = axial force 𝐹𝑦 = Yield force; LCAC in compression or LCAT in tension 𝛼, 𝛽, 𝛾, 𝛿 = Input parameters; must be greater than or equal to 1.1 𝐴, 𝐵 = input paramaters If α, β, γ, δ, A and B are all set to zero then the following default values are used: ALPHA BETA GAMMA DELTA A B = = = = = = 2.0 2.0 2.0 4.0 2.0 -1.0 FOFFS offsets the yield surface parallel to the axial force axis. It is the compressive axial force at which the maximum bending moment capacity about the local s-axis (determined by LCPMS and SFS), and that about the local t-axis (determined by LCPMT and SFT), occur. For steel beams and columns, the value of FOFFS is usually zero. For reinforce concrete beams, columns and shear walls, the maximum bending moment capacity occurs corresponding to a certain compressive axial force, FOFFS. The value of FOFFS can be input as either positive or negative. Internally, LS-DYNA converts FOFFS to, and regards compressive axial force as, negative. Interaction surface FTYPE 4 calculates a utilisation parameter using the yield force and moment data given on card 2, but the elements remain elastic even when the forces or moments exceed yield values. This is done for consistency with the design code OBE AISC LRFD (2000). The utilisation calculation is as follows: Ultilisation = 𝐾1𝐹 𝜙𝐹𝑦 + 𝐾2 𝜙𝑏 ( 𝑀𝑠 𝑀𝑦𝑠 + 𝑀𝑡 𝑀𝑦𝑡 ) where, and, 𝑀𝑠, 𝑀𝑡𝑀𝑦𝑠, 𝑀𝑦𝑡, 𝐹𝑦 are defined as in the preceding equation 𝜙 = from PHI_ T under tension; PHI_ C under compression 𝜙𝑏 = take from PHI_ B 𝐾1 = 0.5 1.0 ⎧ {{{ ⎨ {{{ ⎩ 𝜙𝐹𝑦 𝜙𝐹𝑦 < 0.2 ≥ 0.2 𝐾2 = 1.0 9⁄ ⎧ {{{ ⎨ {{{ ⎩ 𝜙𝐹𝑦 𝜙𝐹𝑦 < 0.2 ≥ 0.2 Interaction surface FTYPE 5 is similar to type 4 (calculates a utilisation parameter using the yield data, but the elements do not yield). The equations are taken from Australian code AS4100. The user must select appropriate values of α, β, γ and δ using the various clauses of Section 8 of AS4100. It is assumed that the local s-axis is the major axis for bending. Utilisation = max(𝑈1, 𝑈2, 𝑈3, 𝑈4, 𝑈5) 𝑈1 = 𝑈2 = 𝛽𝜙𝑐𝐹𝑦𝑐 𝜙𝑡𝐹𝑦𝑡 𝑈3 = [ 𝑈4 = [ 𝑀𝑠 𝐾2𝜙𝑏𝑀𝑦𝑠 𝑀𝑠 𝐾4𝜙𝑏𝑀𝑦𝑠 𝜙𝑐𝐹𝑦𝑐 + ] ] + [ + [ 𝑀𝑠 𝜙𝑏𝑀𝑦𝑠 + 𝑀𝑡 𝐾1𝜙𝑏𝑀𝑦𝑡 𝑀𝑡 𝐾3𝜙𝑏𝑀𝑦𝑡 𝑀𝑡 𝜙𝑏𝑀𝑦𝑡 used for members in compression used for members in tension used for members in compression used for members in tension used for all members ] ] 𝑈5 = where, and, 𝑀𝑠, 𝑀𝑡, 𝐹, 𝑀𝑦𝑠, 𝑀𝑦𝑡, 𝐹𝑦𝑡, 𝐹𝑦𝑐 are as defined above 𝐾1 = 1.0 − 𝛽𝜙𝑐𝐹𝑦𝑐 𝐾2 = min [𝐾1, 𝛼 (1.0 − 𝛿𝜙𝑐𝐹𝑦𝑐 )] 𝐾3 = 1.0 − 𝜙𝑡𝐹𝑦𝑡 𝐾4 = min [K3, 𝛼 (1.0 + 𝜙𝑡𝐹𝑦𝑡 )] where 𝐾1, 𝐾2, 𝐾3𝐾4 are subject to a minimum value of 10−6, 𝛼, 𝛽, 𝛾, 𝛿, 𝜙𝑡, 𝜙𝑐, 𝜙𝑏 are input parameters The option for degrading moment behavior changes the meaning of the plastic moment-rotation curve as follows: If DEGRAD = 0 (not recommended), the x-axis points on the curve represent current plastic rotation (i.e. total rotation minus the elastic component of rotation). This quantity can be positive or negative depending on the direction of rotation; during hysteresis the behavior will repeatedly follow backwards and forwards along the same curve. The curve should include negative and positive rotation and moment values. This option is retained so that results from existing models will be unchanged. If DEGRAD = 1, the x-axis points represent cumulative absolute plastic rotation. This quantity is always positive, and increases whenever there is plastic rotation in either direction. Thus, during hysteresis, the yield moments are taken from points in the input curve with increasingly positive rotation. If the curve shows a degrading behavior (reducing moment with rotation), then, once degraded by plastic rotation, the yield moment can never recover to its initial value. This option can be thought of as having “fatigue-type” hysteretic damage behavior, where all plastic cycles contribute to the total damage. If DEGRAD = 2, the x-axis points represent the high-tide value (always positive) of the plastic rotation. This quantity increases only when the absolute value of plastic rotation exceeds the previously recorded maximum. If smaller cycles follow a larger cycle, the plastic moment during the small cycles will be constant, since the high-tide plastic rotation is not altered by the small cycles. Degrading moment-rotation behavior is possible. This option can be thought of as showing rotation-controlled damage, and follows the FEMA approach for treating fracturing joints. DEGRAD applies also to the axial behavior. The same options are available as for rotation: DEGRAD = 0 gives unchanged behavior from previous versions; DEGRAD = 1 gives a fatigue-type behavior using cumulative plastic strain; and DEGRAD = 2 gives FEMA-type behavior, where the axial load capacity depends on the high-tide tensile and compressive strains. The definition of strain for this purpose is according to AOPT on Card 1 – it is expected that AOPT = 2 will be used with DEGRAD = 2. The “axial strain” variable plotted by post-processors is the variable defined by AOPT. The output variables plotted as “plastic rotation” have special meanings for this material model as follows – note that hinges form only at Node 2: “Plastic rotation at End 1” is really a high-tide mark of absolute plastic rotation at Node 2, defined as follows: 1. Current plastic rotation is the total rotation minus the elastic component of rotation. 2. Take the absolute value of the current plastic rotation, and record the maximum achieved up to the current time. This is the high-tide mark of plastic rotation. If DEGRAD = 0, “Plastic rotation at End 2” is the current plastic rotation at Node 2. If DEGRAD = 1 or 2, “Plastic rotation at End 2” is the current total rotation at Node 2. The total rotation is a more intuitively understood parameter, e.g. for plotting hysteresis loops. However, with DEGRAD = 0, the previous meaning of that output variable has been retained such that results from existing models are unchanged. FEMA thresholds are the plastic rotations at which the element is deemed to have passed from one category to the next, e.g. “Elastic”, “Immediate Occupancy”, “Life Safe”, etc. The high-tide plastic rotation (maximum of Y and Z) is checked against the user-defined limits FEMA1, FEMA2, etc. The output flag is then set to 0, 1, 2, 3, or 4: 0 means that the rotation is less than FEMA1; 1 means that the rotation is between FEMA1 and FEMA2, and so on. By contouring this flag, it is possible to see quickly which joints have passed critical thresholds. For this material model, special output parameters are written to the d3plot and d3thdt files. The number of output parameters for beam elements is automatically increased to 20 (in addition to the six standard resultants) when parts of this material type are present. Some post-processors may interpret this data as if the elements were integrated beams with 4 integration points. Depending on the post-processor used, the data may be accessed as follows: Extra variable 16 (or Integration point 4 Axial Stress): Extra variable 17 (or Integration point 4 XY Shear Stress): Current utilization Extra variable 18 (or Integration point 4 ZX Shear Stress): Maximum utilization FEMA rotation flag to Extra variable 20 (or Integration point 4 Axial Strain): date FEMA axial flag “Utilization” is the yield parameter, where 1.0 is on the yield surface. *MAT_SOIL_BRICK Purpose: This is Material Type 192. It is intended for modeling over-consolidated clay. Card 1 1 2 3 4 5 6 7 8 Variable MID RO RLAMDA RKAPPA RIOTA RBETA1 RBETA2 RMU Type A8 F F F F F F F Default 1.0 Card 2 1 2 3 4 5 6 7 8 Variable RNU RLCID TOL PGCL SUB-INC BLK GRAV THEORY Type F F F F F F F Default 0.0005 9.807 I 0 Additional card for THEORY > 0. Card 3 1 2 3 4 5 6 7 8 Variable RVHHH XSICRIT ALPHA RVH RNU21 ANISO_4 Type Default F 0 F 0 F 0 F 0 F 0 F 0 VARIABLE MID DESCRIPTION Material identification. A unique number or label not exceeding 8 characters must be specified. RO Mass density RLAMDA Material coefficient VARIABLE DESCRIPTION RKAPPA Material coefficient RIOTA Material coefficient RBETA1 Material coefficient RBETA2 Material coefficient RMU Shape factor coefficient. This parameter will modify the shape of the yield surface used. 1.0 implies a von Mises type surface, but 1.1 to 1.25 is more indicative of soils. The default value is 1.0. RNU Poisson’s ratio RLCID TOL PGCL SUB-INC BLK GRAV Load curve identification number referring to a curve defining up to 10 pairs of ‘string-length’ vs G/Gmax points. User defined tolerance for convergence checking. Default value is set to 0.02. Pre-consolidation ground level. This parameter defines the maximum surface level (relative to z = 0.0 in the model) of the soil throughout geological history. This is used calculate the maximum over burden pressure on the soil elements. User defined strain increment size. This is the maximum strain increment that the material model can normally cope with. If the value is exceeded a warning is echoed to the d3hsp file. The elastic bulk stiffness of the soil. This is used for the contact stiffness only. The gravitational acceleration. This is used to calculate the element stresses due the overlying soil. Default is set to 9.807 m/s2. THEORY Version of material subroutines used . EQ.0: 1995 version, vectorized (Default) EQ.4: 2003 version, unvectorized RVHHH Anisotropy ratio Gvh / Ghh (default = Isotropic behavior) XSICRIT Anisotropy parameter *MAT_SOIL_BRICK DESCRIPTION ALPHA Anisotropy parameter RVH Anisotropy ratio Ev / Eh RNU21 Anisotropy ratio 𝜈2/𝜈1 ANISO_4 Anisotropy parameter Remarks: 1. This material type requires that the model is oriented such that the z-axis is defined in the upward direction. Compressive initial stress must be defined, e.g. using *INITIAL_STRESS_SOLID or *INITIAL_STRESS_DEPTH. The recommended unit system is kN, meters, seconds, tonnes. There are some built-in defaults that assume stress units of KN/m2. Over-consolidated clays have suffered previous loading to higher stress levels than are present at the start of the analysis. This could have occurred due to ice sheets during previous ice ages, or the presence of soil or rock that has subse- quently been eroded. The maximum vertical stress during that time is assumed to be: 𝜎VMAX = RO × GRAV × (PGCL − 𝑍el) where RO, GRAV, and PGCL = input parameters 𝑍el = z coordinate of center of element Since that time, the material has been unloaded until the vertical stress equals the user-defined initial vertical stress. The previous load/unload history has a significant effect on subsequent behavior, e.g. the horizontal stress in an over- consolidated clay may be greater than the vertical stress. This material model creates a load/unload cycle for a sample element of each material of this type, stores in a scratch file the horizontal stress and history variables as a function of the vertical stress, and interpolates these quantities from the defined initial vertical stress for each element. Therefore the initial horizontal stress seen in the output files will be different from the input initial horizontal stress. This material model is developed for a Geotechnical FE program (Oasys Ltd.’s SAFE) written by Arup. The default THEORY = 0 gives a vectorized version ported from SAFE in the 1990’s. Since then the material model has been devel- oped further in SAFE; the most recent porting is accessed using THEORY = 4 (recommended); however, this version is not vectorized and will run more slowly on most computer platforms. 2. The shape factor for a typical soil would be 1.25. Do not use values higher than 1.35. *MAT_DRUCKER_PRAGER Purpose: This is Material Type 193. This material enables soil to be modeled effectively. The parameters used to define the yield surface are familiar geotechnical parameters (i.e. angle of friction). The modified Drucker-Prager yield surface is used in this material model enabling the shape of the surface to be distorted into a more realistic definition for soils. Card 1 1 2 3 4 5 6 7 8 Variable MID RO GMOD RNU RKF PHI CVAL PSI Type A8 F F F F F F F Default 1.0 0.0 Card 2 1 2 3 4 5 6 7 8 Variable STR_LIM Type F Default 0.005 Card 3 1 2 3 4 5 6 7 8 Variable GMODDP PHIDP CVALDP PSIDP GMODGR PHIGR CVALGR PSIGR Type F F F F F F F F Default 0.0 0.0 0.0 0.0 0.0 0.0 0.0 0.0 VARIABLE MID DESCRIPTION Material identification. A unique number or label not exceeding 8 characters must be specified. RO Mass density VARIABLE DESCRIPTION GMOD Elastic shear modulus RNU RKF PHI Poisson’s ratio Failure surface shape parameter Angle of friction (radians) CVAL Cohesion value PSI Dilation angle (radians) STR_LIM Minimum shear strength of material is given by STR_LIM*CVAL GMODDP Depth at which shear modulus (GMOD) is correct PHIDP Depth at which angle of friction (PHI) is correct CVALDP Depth at which cohesion value (CVAL) is correct PSIDP Depth at which dilation angle (PSI) is correct GMODGR Gradient at which shear modulus (GMOD) increases with depth PHIGR Gradient at which friction angle (PHI) increases with depth CVALGR Gradient at which cohesion value (CVAL) increases with depth PSIGR Gradient at which dilation angle (PSI) increases with depth Remarks: 1. This material type requires that the model is oriented such that the z-axis is defined in the upward direction. The key parameters are defined such that may vary with depth (i.e. the z-axis). 2. The shape factor for a typical soil would be 0.8, but should not be pushed further than 0.75. 3. If STR_LIM is set to less than 0.005, the value is reset to 0.005. 4. The yield function is defined as: t – p.tanβ – d = 0 where: p = hydrostatic stress = J1/3 t = (q/2){a – b(r/q)3} q = Von Mises stress = √(3J2) a = 1 + 1/K b = 1 – 1/K K = input parameter RKF r = (27 J3/2)1/3 J2,J3 = second and third deviatoric stress invariants tanβ = 6 sinφ / (3-sinφ) d = 6 C cosφ / (3-sinφ) φ= input parameter PHI C = input parameter CVAL *MAT_194 Purpose: This is Material Type 194. It is for shell elements only. It uses empirically- derived algorithms to model the effect of cyclic shear loading on reinforced concrete walls. It is primarily intended for modeling squat shear walls, but can also be used for slabs. Because the combined effect of concrete and reinforcement is included in the empirical data, crude meshes can be used. The model has been designed such that the minimum amount of input is needed: generally, only the variables on the first card need to be defined. NOTE: This material does not support specification of a ma- terial angle, 𝛽𝑖, for each through-thickness integra- tion point of a shell. Card 1 1 Variable MID 2 RO Type A8 F 3 E F 4 PR F 5 6 7 TMAX F 8 I Default none none none 0.0 0.0 Include the following data if “Uniform Building Code” formula for maximum shear strength or tensile cracking are required – otherwise leave blank. Card 2 Variable 1 FC 2 3 4 5 6 PREF FYIELD SIG0 UNCONV ALPHA Type F F F F F F 7 FT F 8 ERIENF F Default 0.0 0.0 0.0 0.0 0.0 0.0 0.0 0.0 Variable Type 1 A F *MAT_RC_SHEAR_WALL 2 B F 3 C F 4 D F 5 E F 6 F F 7 8 Default 0.05 0.55 0.125 0.66 0.25 1.0 Card 4 Variable 1 Y1 Type F 2 Y2 F 3 Y3 F 4 Y4 F 5 Y5 F Default 0.0 0.0 0.0 0.0 0.0 Card 5 Variable 1 T1 Type F 2 T2 F 3 T3 F 4 T4 F 5 T5 F Default 0.0 0.0 0.0 0.0 0.0 6 7 8 6 7 8 Card 6 1 2 3 4 5 6 7 8 Variable AOPT Type F Default 0.0 Variable 1 XP Type F 2 YP F 3 ZP F 4 A1 F 5 A2 F 6 A3 F Default 0.0 0.0 0.0 0.0 0.0 0.0 *MAT_194 7 8 Card 8 Variable 1 V1 Type F 2 V2 F 3 V3 F 4 D1 F 5 D2 F 6 D3 F 7 8 BETA F Default 0.0 0.0 0.0 0.0 0.0 0.0 0.0 VARIABLE DESCRIPTION MID RO E PR TMAX FC Material identification. A unique number or label not exceeding 8 characters must be specified. Mass density Young’s Modulus Poisson’s Ratio Ultimate in-plane shear stress. If set to zero, LS-DYNA will calculate TMAX based on the formulae in the Uniform Building Code, using the data on card 2. See Remarks. Unconfined Compressive Strength of concrete (used in the calculation of ultimate shear stress; crushing behavior is not modeled) PREF Percent reinforcement, e.g. if 1.2% reinforcement, enter 1.2 FYIELD Yield stress of reinforcement SIG0 Overburden stress (in-plane compressive stress) - used in the calculation of ultimate shear stress. Usually sig0 is left as zero. *MAT_RC_SHEAR_WALL DESCRIPTION UCONV Unit conversion factor. UCONV is expected to be set such that, UCONV = √1.0 PSI in the model's stress units. This used to convert the ultimate tensile stress of concrete which is expressed as √FC where FC is given in PSI. Therefore a unit conversion factor of √PSI Stress Unit is required. Examples: ⁄ UCONV = 83.3 = √6894 if stress unit is N/m2 UCONV = 0.083 if stress unit is MN/m2 or N/mm2 ALPHA Shear span factor - see below. FT ERIENF A B C D E F Cracking stress in direct tension - see notes below. Default is 8% of the cylinder strength. Young’s Modulus of reinforcement. Used in calculation of post- cracked stiffness - see notes below. Hysteresis constants determining the shape of the hysteresis loops. Hysteresis constants determining the shape of the hysteresis loops. Hysteresis constants determining the shape of the hysteresis loops. Hysteresis constants determining the shape of the hysteresis loops. Hysteresis constants determining the shape of the hysteresis loops. Strength degradation factor. After the ultimate shear stress has been achieved, F multiplies the maximum shear stress from the curve for subsequent reloading. F = 1.0 implies no strength degradation (default). F = 0.5 implies that the strength is halved for subsequent reloading. Y1, Y2, …, Y5 Engineering shear strain points on stress-strain curve. By default these are calculated from the values on card 1. See below for more guidance. VARIABLE T1, T2, …, T5 DESCRIPTION Shear stress points on stress-strain curve. By default these are calculated from the values on card 1. See below for more guidance. AOPT Material axes option: EQ.0.0: locally orthotropic with material axes determined by element nodes as shown in Figure M2-1, and then ro- tated about the shell element normal by the angle BE- TA. Nodes 1, 2, and 4 of an element are identical to the nodes used for the definition of a coordinate system as by *DEFINE_COORDINATE_NODES. EQ.2.0: globally orthotropic with material axes determined by vectors defined below, as with *DEFINE_COORDI- NATE_VECTOR. EQ.3.0: applicable to shell elements only. This option determines locally orthotropic material axes by offset- ting the material axes by an angle to be specified from a line in the plane of the shell determined by taking the cross product of the vector v defined below with the shell normal vector. LT.0.0: the absolute value of AOPT is a coordinate system ID number (CID on *DEFINE_COORDINATE_NODES, *DEFINE_COORDINATE_SYSTEM or *DEFINE_CO- ORDINATE_VECTOR). Available in R3 version of 971 and later. XP, YP, ZP Coordinates of point 𝐩 for AOPT = 1. A1, A2, A3 Components of vector 𝐚 for AOPT = 2. V1, V2, V3 Components of vector 𝐯 for AOPT = 3. D1, D2, D3 Components of vector 𝐝 for AOPT = 2. BETA Material angle in degrees for AOPT = 0 and 3, may be overridden on the element card, see *ELEMENT_SHELL_BETA. Remarks: The element is linear elastic except for in-plane shear and tensile cracking effects. Crushing due to direct compressive stresses are modeled only insofar as there is an in- plane shear stress component. It is not recommended that this model be used where nonlinear response to direct compressive or loads is important. Note that the in-plane shear stress 𝑡𝑥𝑦 is defined as the shear stress in the element’s local 𝑥-𝑦 plane. This is not necessarily equal to the maximum shear stress in the plane: for example, if the principal stresses are at 45 degrees to the local axes, 𝑡𝑥𝑦 is zero. Therefore it is important to ensure that the local axes are appropriate - for a shear wall the local axes should be vertical or horizontal. By default, local 𝑥 points from node 1 to node 2 of the element. It is possible to change the local axes by using AOPT > 0. If TMAX is set to zero, the ultimate shear stress is calculated using a formula in the Uniform Building Code 1997, section 1921.6.5: TMAXUBC = UCONV × ALPHA × √FC + RO × FY where, UCONV = unit conversion factor, see varriable list ALPHA = aspect ratio = 2.0 for ℎ 𝑙⁄ ∈ (2.0, ∞) increases linearly to 3.0 for ℎ 𝑙⁄ ∈ (2.0,1.5) FC = unconfined compressive strength of concrete RO = fraction of reinforcement = (percent reinforcement) 100 ⁄ FY = yield stress of reinforcement To this we add shear stress due to the overburden to obtain the ultimate shear stress: TMAXUBC = TMAXUBC + SIG0 where SIG0 = in plane compressive stress under static equilibrium conditions The UBC formula for ultimate shear stress is generally conservative (predicts that the wall is weaker than shown in test), sometimes by 50% or more. A less conservative formula is that of Fukuzawa: TMAX = max [(0.4 + 𝐴𝑐 𝐴𝑤 ) , 1] × 2.7 × (1.9 + 𝐿𝑣 ) × UCONV+√FC + 0.5 × RO × FY + SIG0 where 𝐴𝐶 = Cross-sectional area of stiffening features such as columns or flanges 𝐴𝑤 = Cross-sectional area of wall ⁄ 𝑀 𝐿𝑣⁄ = Aspect ratio of wall height length Other terms are as above. This formula is not included in the material model: TMAX should be calculated by hand and entered on Card 1 if the Fukuzawa formula is required. It should be noted that none of the available formulae, including Fukuzawa, predict the ultimate shear stress accurately for all situations. Variance from the experimental results can be as great as 50%. The shear stress vs shear strain curve is then constructed automatically as follows, using the algorithm of Fukuzawa extended by Arup: 1. Assume ultimate engineering shear strain, 𝛾𝑢 = 0.0048 2. First point on curve, corresponding to concrete cracking, is at (0.3 × TMAX , 0.3 × TMAX), where 𝐺 is the elastic shear modulus given by 𝐺 = 2(1 + 𝜈) . 3. Second point, corresponding to the reinforcement yield, is at 4. Third point, corresponding to the ultimate strength, is at (0.5 × 𝛾𝑢, 0.8 × TMAX). (𝛾𝑢, TMAX). 5. Fourth point, corresponding to the onset of strength reduction, is at 6. Fifth point, corresponding to failure is at (2𝛾𝑢,TMAX). (3𝛾𝑢, 0.6 × TMAX). After failure, the shear stress drops to zero. The curve points can be entered by the user if desired, in which case they over-ride the automatically calculated curve. However, it is anticipated that in most cases the default curve will be preferred due to ease of input. Hysteresis follows the algorithm of Shiga as for the squat shear wall spring . The hysteresis constants which are defined in fields A, B, C, D, and E can be entered by the user if desired, but it is generally recommended that the default values be used. Cracking in tension is checked for the local x and y directions only – this is calculated separately from the in-plane shear. A trilinear response is assumed, with turning points at concrete cracking and reinforcement yielding. The three regimes are: 1. Pre-cracking, linear elastic response is assumed using the overall Young’s Modulus on Card 1. 2. Cracking occurs in the local x or y directions when the tensile stress in that direction exceeds the concrete tensile strength FT (if not input on Card 2, this defaults to 8% of the compressive strength FC). Post-cracking, a linear stress- strain response is assumed up to reinforcement yield at a strain defined by reinforcement yield stress divided by reinforcement Young’s Modulus. 3. Post-yield, a constant stress is assumed (no work hardening). Unloading returns to the origin of the stress-strain curve. For compressive strains the response is always linear elastic using the overall Young’s Modulus on Card 1. If insufficient data is entered, no cracking occurs in the model. As a minimum, FC and FY are needed. Extra variables are available for post-processing as follows: Extra variable 1: Current engineering shear strain Extra variable 2: Shear status: 0, 1, 2, 3, 4, or 5– see below Extra variable 3: Maximum direct strain so far in local 𝑥 direction (for ten- sile cracking) Extra variable 4: Maximum direct strain so far in local 𝑦 direction (for ten- sile cracking) Extra variable 5: Tensile status: 0, 1 or 2 = elastic, cracked, or yielded re- spectively. The shear status shows how far along the shear stress-strain curve each element has progressed, e.g. status 2 means that the element has passed the second point on the curve. These status levels correspond to performance criteria in building design codes such as FEMA. *MAT_195 This is Material Type 195 for beam elements. An elasto-plastic material with an arbitrary stress versus strain curve and arbitrary strain rate dependency can be defined. See also Remark below. Also, failure based on a plastic strain or a minimum time step size can be defined. Card 1 1 Variable MID 2 RO Type A8 F 3 E F 4 PR F 5 6 7 8 SIGY ETAN FAIL TDEL F F F F Default none none none none none 0.0 10.E+20 10.E+20 Card 2 Variable Type Default 1 C F 0 Card 3 1 2 P F 0 2 3 4 5 6 7 8 LCSS LCSR F 0 3 F 0 4 5 6 7 8 Variable NOTEN TENCUT SDR Type Default I 0 F F E15.0 0.0 VARIABLE MID DESCRIPTION Material identification. A unique number or label not exceeding 8 characters must be specified. RO Mass density. E PR SIGY ETAN FAIL *MAT_CONCRETE_BEAM DESCRIPTION Young’s modulus. Poisson’s ratio. Yield stress. Tangent modulus, ignored if (LCSS.GT.0) is defined. Failure flag. LT.0.0: user defined failure subroutine is called to determine failure EQ.0.0: failure is not considered. This option is recommended if failure is not of interest since many calculations will be saved. GT.0.0: plastic strain to failure. When the plastic strain reaches this value, the element is deleted from the calculation. TDEL Minimum time step size for automatic element deletion. C P LCSS Strain rate parameter, C, see formula below. Strain rate parameter, P, see formula below. Load curve ID or Table ID. Load curve ID defining effective stress versus effective plastic strain. If defined EPS1-EPS8 and ES1-ES8 are ignored. The table ID defines for each strain rate value a load curve ID giving the stress versus effective plastic strain for that rate, See Figure M16-1 stress versus effective plastic strain curve for the lowest value of strain rate is used if the strain rate falls below the minimum value. Likewise, the stress versus effective plastic strain curve for the highest value of strain rate is used if the strain rate exceeds the maximum value. The strain rate parameters: C and P; LCSR Load curve ID defining strain rate scaling effect on yield stress. NOTEN No-tension flag, EQ.0: beam takes tension, EQ.1: beam takes no tension, EQ.2: beam takes tension up to value given by TENCUT. TENCUT Tension cutoff value. VARIABLE DESCRIPTION SDR Stiffness degradation factor. Remarks: The stress strain behavior may be treated by a bilinear stress strain curve by defining the tangent modulus, ETAN. An effective stress versus effective plastic strain curve (LCSS) may be input instead of defining ETAN. The cost is roughly the same for either approach. The most general approach is to use the table definition (LCSS) discussed below. Three options to account for strain rate effects are possible. 1. Strain rate may be accounted for using the Cowper and Symonds model which scales the yield stress with the factor 1 + ( 𝑝⁄ ) 𝜀̇ where 𝜀̇ is the strain rate. 𝜀̇ = √𝜀̇𝑖𝑗𝜀̇𝑖𝑗. 2. For complete generality a load curve (LCSR) to scale the yield stress may be input instead. In this curve the scale factor versus strain rate is defined. 3. If different stress versus strain curves can be provided for various strain rates, the option using the reference to a table (LCSS) can be used. *MAT_GENERAL_SPRING_DISCRETE_BEAM This is Material Type 196. This model permits elastic and elastoplastic springs with damping to be represented with a discrete beam element of type 6 by using six springs each acting about one of the six local degrees-of-freedom. For elastic behavior, a load curve defines force or moment versus displacement or rotation. For inelastic behavior, a load curve defines yield force or moment versus plastic deflection or rotation, which can vary in tension and compression. The two nodes defining a beam may be coincident to give a zero length beam, or offset to give a finite length beam. For finite length discrete beams the absolute value of the variable SCOOR in the SECTION_BEAM input should be set to a value of 2.0, which causes the local r-axis to be aligned along the two nodes of the beam to give physically correct behavior. The distance between the nodes of a beam should not affect the behavior of this material model. A triad is used to orient the beam for the directional springs. 3 4 5 6 7 8 Card 1 1 Variable MID 2 RO Type A8 F Degree of Freedom Card Pairs. For each active degree of freedom include a pair of cards 2 and 3. This data is terminated by the next keyword (“*”) card or when all six degrees of freedom have been specified. Card 2 1 2 Variable DOF TYPE Type I Card 3 1 I 2 Variable FLCID HLCID Type F F 3 K F 3 C1 F 4 D F 4 C2 F 5 6 7 8 CDF TDF F 5 F 6 DLE GLCID F I 7 VARIABLE DESCRIPTION MID RO DOF Material identification. A unique number or label not exceeding 8 characters must be specified. Mass density, see also volume in *SECTION_BEAM definition. Active degree-of-freedom, a number between 1 and 6 inclusive. Each value of DOF can only be used once. The active degree-of- freedom is measured in the local coordinate system for the discrete beam element. TYPE The default behavior is elastic. For inelastic behavior input 1. K D CDF TDF FLCID Elastic loading/unloading stiffness. This is required input for inelastic behavior. Optional viscous damping coefficient. Compressive displacement at failure. Input as a positive number. After failure, no forces are carried. This option does not apply to zero length springs. EQ.0.0: inactive. Tensile displacement at failure. After failure, no forces are carried. EQ.0.0: inactive. Load curve ID, see *DEFINE_CURVE. For option TYPE = 0, this curve defines force or moment versus deflection for nonlinear elastic behavior. For option TYPE = 1, this curve defines the yield force versus plastic deflection. If the abscissa of the first point of the curve is 0. the force magnitude is identical in tension and compression, i.e., only the sign changes. If not, the yield stress in the compression is used when the spring force is negative. The plastic displacement increases monotonically in this implementa- tion. The load curve is required input. HLCID Load curve ID, see *DEFINE_CURVE, defining force versus relative velocity (Optional). If the origin of the curve is at (0,0) the force magnitude is identical for a given magnitude of the relative velocity, i.e., only the sign changes. C1 C2 Damping coefficient. Damping coefficient *MAT_GENERAL_SPRING_DISCRETE_BEAM DESCRIPTION DLE Factor to scale time units. GLCID Optional load curve ID, see *DEFINE_CURVE, defining a scale factor versus deflection for load curve ID, HLCID. If zero, a scale factor of unity is assumed. Remarks: If TYPE = 0, elastic behavior is obtained. In this case, if the linear spring stiffness is used, the force, F, is given by: 𝐹 = K × Δ𝐿 + D × Δ𝐿̇ but if the load curve ID is specified, the force is then given by: 𝐹 = 𝐾 𝑓 (Δ𝐿) [1 + C1 × Δ𝐿̇ + C2 × sgn(Δ𝐿̇)ln (max {1. , ∣Δ𝐿̇∣ DLE })] + D×Δ𝐿̇ + 𝑔(Δ𝐿)ℎ(Δ𝐿̇) In these equations, Δ𝐿 is the change in length Δ𝐿 = current length − initial length For the first three degrees of freedom the parameters on cards 2 and 3 have dimensions as shown below. Being angular in nature, the next three degrees of freedom involve moment instead of force and angle instead of length, but are otherwise identical. [K] = [D] = ⎧ [force] { [length] ⎨ { ⎩ unitless [force] [velocity] FLCID = 0 FLCID > 0 [force][time] [length] = [FLCID] = [GLCID] = ([length], [force]) [HLCID] = ([velocity], [force]) [C1] = [time] [length] [C2] = unitless [DLE] = [length] [time] If TYPE = 1, inelastic behavior is obtained. In this case, the yield force is taken from the load curve: 𝐹𝑌 = 𝐹𝑦(Δ𝐿plastic) where 𝐿plastic is the plastic deflection. A trial force is computed as: and is checked against the yield force to determine 𝐹: 𝐹𝑇 = 𝐹𝑛 + K × Δ𝐿̇(Δ𝑡) 𝐹 = {𝐹𝑌 𝐹𝑇 if 𝐹𝑇 > 𝐹𝑌 if 𝐹𝑇 ≤ 𝐹𝑌 The final force, which includes rate effects and damping, is given by: 𝐹𝑛+1 = 𝐹 × [1 + C1 × Δ𝐿̇ + C2 × sgn(Δ𝐿̇)ln (max {1. , ∣Δ𝐿̇∣ DLE })] + D × Δ𝐿̇ + 𝑔(Δ𝐿)ℎ(Δ𝐿̇) Unless the origin of the curve starts at (0,0), the negative part of the curve is used when the spring force is negative where the negative of the plastic displacement is used to interpolate, 𝐹𝑦. The positive part of the curve is used whenever the force is positive. The cross sectional area is defined on the section card for the discrete beam elements, See *SECTION_BEAM. The square root of this area is used as the contact thickness offset if these elements are included in the contact treatment. *MAT_SEISMIC_ISOLATOR This is Material Type 197 for discrete beam elements. Sliding (pendulum) and elastomeric seismic isolation bearings can be modeled, applying bi-directional coupled plasticity theory. The hysteretic behavior was proposed by Wen [1976] and Park, Wen, and Ang [1986]. The sliding bearing behavior is recommended by Zayas, Low and Mahin [1990]. The algorithm used for implementation was presented by Nagarajaiah, Reinhorn, and Constantinou [1991]. Further options for tension-carrying friction bearings are as recommended by Roussis and Constantinou [2006]. Element formulation type 6 must be used. Local axes are defined on *SECTION_BEAM; the default is the global axis system. It is expected that the local z-axis will be vertical. On *SECTION_BEAM SCOOR must be set to zero when using this material model. Card 1 1 Variable MID 2 RO Type A8 F 3 A F 4 5 6 7 8 BETA GAMMA DISPY STIFFV ITYPE F F F F I Default none none 1.0 0.5 0.5 0.0 0.0 0.0 Card 2 1 2 3 4 5 6 7 8 Variable PRELOAD DAMP MX1 MX2 MY1 MY2 Type Default F 0 F 1.0 F 0 F 0 F 0 F Sliding Isolator Card. This card is used for ITYPE = 0 or 2. Leave this card blank for elastomeric isolator (TYPE = 1). Card 3 1 2 3 4 5 6 7 8 Variable FMAX DELF AFRIC RADX RADY RADB STIFFL STIFFTS Type Default F 0 F 0 F 0 F F F F 1.0e20 1.0e20 1.0e20 STIFFV F 0 Card 4 for ITYPE = 1 or 2. leave blank for sliding isolator ITYPE = 0: Card 4 1 2 3 4 5 6 7 8 Variable FORCEY ALPHA STIFFT DFAIL FMAXYC FMAXXT FMAXYT YLOCK Type Default F 0 F 0 F F F F F F 0.5 × STIFFV 1.0e20 FMAX FMAX FMAX 0.0 VARIABLE DESCRIPTION MID RO A Material identification. A unique number or label not exceeding 8 characters must be specified. Mass density. Nondimensional variable - see below GAMMA Nondimensional variable - see below BETA DISPY Nondimensional variable - see below Yield displacement (length units - must be > 0.0) STIFFV Vertical stiffness (force/length units) ITYPE Type: *MAT_SEISMIC_ISOLATOR DESCRIPTION EQ.0: sliding (spherical or cylindrical) EQ.1: elastomeric EQ.2: sliding (two perpendicular curved beams) PRELOAD Vertical preload not explicitly modeled (force units) DAMP Damping ratio (nondimensional) MX1, MX2 Moment factor at ends 1 and 2 in local X-direction MY1, MY2 Moment factor at ends 1 and 2 in local Y-direction FMAX Maximum friction coefficient (dynamic) DELF Difference between maximum coefficient friction and static friction AFRIC Velocity multiplier in sliding friction equation (time/length units) RADX RADY RADB Radius for sliding in local X direction Radius for sliding in local Y direction Radius of retaining ring STIFFL Stiffness for lateral contact against the retaining ring STIFFTS Stiffness for tensile vertical response (sliding isolator - default = 0) FORCEY ALPHA STIFFT DFAIL Yield force. Used for elastomeric type (ITYPE = 1). Leave blank for sliding type (0, and 2). Ratio of postyielding stiffness to preyielding stiffness. Used for elastomeric type (ITYPE = 1). Leave blank for sliding type (0, and 2). Stiffness for tensile vertical response (elastomeric isolator). Used for elastomeric type (ITYPE = 1). Leave blank for sliding type (0, and 2). Lateral displacement at which the isolator fails. Used for elastomeric type (ITYPE = 1). Leave blank for sliding type (0, and 2). DESCRIPTION Max friction coefficient (dynamic) for local Y-axis (compression). Used for ITYPE = 2. Leave blank for ITYPE = 0 or 1. Max friction coefficient (dynamic) for local X-axis (tension). Used for ITYPE = 2. Leave blank for ITYPE = 0 or 1. Max friction coefficient (dynamic) for local Y-axis (tension). Used for ITYPE = 2. Leave blank for ITYPE = 0 or 1. Stiffness locking the local Y-displacement (optional -single-axis sliding). Used for ITYPE = 2. Leave blank for ITYPE = 0 or 1. VARIABLE FMAXYC FMAXXT FMAXYT YLOCK Remarks: The horizontal behavior of both types is governed by plastic history variables Zx, Zy that evolve according to equations given in the reference; A, gamma and beta and the yield displacement are the input parameters for this. The intention is to provide smooth build-up, rotation and reversal of forces in response to bidirectional displacement histories in the horizontal plane. The theoretical model has been correlated to experiments on seismic isolators. The RADX, RADY inputs for the sliding isolator are optional. If left blank, the sliding surface is assumed to be flat. A cylindrical surface is obtained by defining either RADX or RADY; a spherical surface can be defined by setting RADX = RADY. The effect of the curved surface is to add a restoring force proportional to the horizontal displacement from the center. As seen in elevation, the top of the isolator will follow a curved trajectory, lifting as it displaces away from the center. The vertical behavior for all types is linear elastic, but with different stiffnesses for tension and compression. By default, the tensile stiffness is zero for the sliding types. The vertical behavior for the elastomeric type is linear elastic; in the case of uplift, the tensile stiffness will be different to the compressive stiffness. For the sliding type, compression is treated as linear elastic but no tension can be carried. Vertical preload can be modeled either explicitly (for example, by defining gravity), or by using the PRELOAD input. PRELOAD does not lead to any application of vertical force to the model. It is added to the compression in the element before calculating the friction force and tensile/compressive vertical behavior. ITYPE = 0 is used to model a single (spherical) pendulum bearing. Triple pendulum bearings can be modelled using three of these elements in series, following the method described by Fenz and Constantinou 2008. The input properties for the three elements (given by⎯Reff1,⎯μ1,⎯d1, ⎯a1, etc) are calculated from the properties of the actual triple bearing (given by Reff1, μ1, d1, a1, etc) as follows: ITYPE = 2 is intended to model uplift-prevention sliding isolators that consist of two perpendicular curved beams joined by a connector that can slide in slots on both beams. The beams are aligned in the local X and Y axes respectively. The vertical displacement is the sum of the displacements induced by the respective curvatures and slider displacements along the two beams. Single-axis sliding is obtained by using YLOCK to lock the local-Y displacement. To resist uplift, STIFFTS must be defined (recommended value: same as STIFFV). This isolator type allows different friction coefficients on each beam, and different values in tension and compression. The total friction, taking into account sliding velocity and the friction history functions, is first calculated using FMAX and then scaled by FMAXXT/FMAX etc as appropriate. For this reason, FMAX should not be zero. DAMP is the fraction of critical damping for free vertical vibration of the isolator, based on the mass of the isolator (including any attached lumped masses) and its vertical stiffness. The viscosity is reduced automatically if it would otherwise infringe numerical stability. Damping is generally recommended: oscillations in the vertical force would have a direct effect on friction forces in sliding isolators; for isolators with curved surfaces, vertical oscillations can be excited as the isolator slides up and down the curved surface. It may occasionally be necessary to increase DAMP if these oscillations become significant. This element has no rotational stiffness - a pin joint is assumed. However, if required, moments can be generated according to the vertical load multiplied by the lateral displacement of the isolator. The moment about the local X-axis (i.e. the moment that is dependent on lateral displacement in the local Y-direction) is reacted on nodes 1 and 2 of the element in the proportions MX1 and MX2 respectively. Similarly, moments about the local Y-axis are reacted in the proportions MY1, MY2. These inputs effectively determine the location of the pin joint. For example, a pin at the base of the column could be modeled by setting MX1 = MY1 = 1.0, MX2 = MY2 = 0.0 and ensuring that node 1 is on the foundation, node 2 at the base of the column - then all the moment is transferred to the foundation. For the same model, MX1 = MY1 = 0.0, MX2 = MY2 = 1.0 would imply a pin at the top of the foundation - all the moment is transferred to the column. Some isolator designs have the pin at the bottom for moments about one horizontal axis, and at the top for the other axis - these can be modeled by setting MX1 = MY2 = 1.0, MX2 = MY1 = 0.0. It is expected that all MX1,2, etc lie between 0 and 1, and that MX1+MX2 = 1.0 (or both can be zero) - e.g. MX1 = MX2 = 0.5 is permitted - but no error checks are performed to ensure this; similarly for MY1 + MY2. Density should be set to a reasonable value, say 2000 to 8000 kg/m3. The element mass will be calculated as density x volume (volume is entered on *SECTION_BEAM). Note on values for *SECTION_BEAM: 1. Set ELFORM to 6 (discrete beam) 2. VOL (the element volume) might typically be set to 0.1m3 3. INER needs to be non-zero (say 1.0) but the value has no effect on the solution since the element has no rotational stiffness. 4. CID can be left blank if the isolator is aligned in the global coordinate system, otherwise a coordinate system should be referenced. 5. By default, the isolator will be assumed to rotate with the average rotation of its two nodes. If the base of the column rotates slightly the isolator will no longer be perfectly horizontal: this can cause unexpected vertical displacements cou- pled with the horizontal motion. To avoid this, rotation of the local axes of the isolator can be eliminated by setting RRCON, SRCON and TRCON to 1.0. This does not introduce any rotational restraint to the model, it only prevents the orientation of the isolator from changing as the model deforms. 6. SCOOR must be set to zero. 7. All other parameters on *SECTION_BEAM can be left blank. Post-processing note: as with other discrete beam material models, the force described in post-processors as “Axial” is really the force in the local X-direction; “Y-Shear” is really the force in the local Y-direction; and “Z-Shear” is really the force in the local Z- direction. *MAT_JOINTED_ROCK This is Material Type 198. Joints (planes of weakness) are assumed to exist throughout the material at a spacing small enough to be considered ubiquitous. The planes are assumed to lie at constant orientations defined on this material card. Up to three planes can be defined for each material. See *MAT_MOHR_COULOMB (*MAT_173) for a preferred alternative to this material model. Card 1 1 2 3 4 5 6 7 8 Variable MID RO GMOD RNU RKF PHI CVAL PSI Type A8 F F F F F F F Default 1.0 0.0 Card 2 1 2 3 4 5 6 7 8 Variable STR_LIM NPLANES ELASTIC LCCPDR LCCPT LCCJDR LCCJT LCSFAC Type F Default 0.005 Card 3 1 I 0 2 I 0 3 I 0 4 I 0 5 I 0 6 I 0 7 I 0 8 Variable GMODDP PHIDP CVALDP PSIDP GMODGR PHIGR CVALGR PSIGR Type F F F F F F F F Default 0.0 0.0 0.0 0.0 0.0 0.0 0.0 0.0 Repeat Card 4 for each plane (maximum 3 planes): Card 4 1 2 3 4 5 6 7 8 Variable DIP STRIKE CPLANE FRPLANE TPLANE SHRMAX LOCAL Type F F F F F F F Default 0.0 0.0 0.0 0.0 0.0 1.e20 0.0 VARIABLE MID DESCRIPTION Material identification. A unique number or label not exceeding 8 characters must be specified. RO Mass density GMOD Elastic shear modulus RNU RKF PHI Poisson’s ratio Failure surface shape parameter Angle of friction (radians) CVAL Cohesion value PSI Dilation angle (radians) STR_LIM Minimum shear strength of material is given by STR_LIM*CVAL NPLANES Number of joint planes (maximum 3) ELASTIC Flag = 1 for elastic behavior only LCCPDR Load curve for extra cohesion for parent material (dynamic relaxation) LCCPT Load curve for extra cohesion for parent material (transient) LCCJDR Load curve for extra cohesion for joints (dynamic relaxation) LCCJT Load curve for extra cohesion for joints (transient) LCSFAC Load curve giving factor on strength vs time *MAT_JOINTED_ROCK DESCRIPTION GMODDP Depth at which shear modulus (GMOD) is correct PHIDP Depth at which angle of friction (PHI) is correct CVALDP Depth at which cohesion value (CVAL) is correct PSIDP Depth at which dilation angle (PSI) is correct GMODGR Gradient at which shear modulus (GMOD) increases with depth PHIGR Gradient at which friction angle (PHI) increases with depth CVALGR Gradient at which cohesion value (CVAL) increases with depth PSIGR Gradient at which dilation angle (PSI) increases with depth DIP Angle of the plane in degrees below the horizontal DIPANG Plan view angle (degrees) of downhill vector drawn on the plane CPLANE Cohesion for shear behavior on plane PHPLANE Friction angle for shear behavior on plane (degrees) TPLANE Tensile strength across plane (generally zero or very small) SHRMAX Max shear stress on plane (upper compression) limit, independent of LOCAL EQ.0: DIP and DIPANG are with respect to the global axes Remarks: 1. The joint plane orientations are defined by the angle of a “downhill vector” drawn on the plane, i.e. the vector is oriented within the plane to obtain the maximum possible downhill angle. DIP is the angle of this line below the hori- zontal. DIPANG is the plan-view angle of the line (pointing down hill) meas- ured clockwise from the global Y-axis about the global Z-axis. 2. The joint planes rotate with the rigid body motion of the elements, irrespective of whether their initial definitions are in the global or local axis system. 3. The full facilities of the modified Drucker Prager model for the matrix material can be used – see description of Material type 193. Alternatively, to speed up the calculation, the ELASTIC flag can be set to 1, in which case the yield surface will not be considered and only RO, GMOD, RNU, GMODDP, GMODGR and the joint planes will be used. 4. This material type requires that the model is oriented such that the z-axis is defined in the upward direction. The key parameters are defined such that may vary with depth (i.e. the z-axis) 5. The shape factor for a typical soil would be 0.8, but should not be pushed further than 0.75. 6. If STR_LIM is set to less than 0.005, the value is reset to 0.005. 7. A correction has been introduced into the Drucker Prager model, such that the yield surface never infringes the Mohr-Coulomb criterion. This means that the model does not give the same results as a “pure” Drucker Prager model. 8. The load curves LCCPDR, LCCPT, LCCJDR, LCCJT allow additional cohesion to be specified as a function of time. The cohesion is additional to that specified in the material parameters. This is intended for use during the initial stages of an analysis to allow application of gravity or other loads without cracking or yielding, and for the cracking or yielding then to be introduced in a controlled manner. This is done by specifying extra cohesion that exceeds the expected stresses initially, then declining to zero. If no curves are specified, no extra cohesion is applied. 9. The load curve for factor on strength applies simultaneously to the cohesion and tan (friction angle) of parent material and all joints. This feature is intend- ed for reducing the strength of the material gradually, to explore factors of safety. If no curve is present, a constant factor of 1 is assumed. Values much greater than 1.0 may cause problems with stability. 10. Extra variables for plotting. By setting NEIPH on *DATABASE_EXTENT_BI- NARY to 15, the following variables can be plotted in D3PLOT and T/HIS: Extra Variable 1: mobilized strength fraction for base material Extra Variable 2: Extra Variable 3: Extra Variable 4: Extra Variable 5: Extra Variable 6: Extra Variable 7: Extra Variable 8: Extra Variable 9: Extra Variable 10: current shear utilization for plane 1 Extra Variable 11: current shear utilization for plane 2 Extra Variable 12: current shear utilization for plane 3 rk0 for base material rlamda for base material crack opening strain for plane 1 crack opening strain for plane 2 crack opening strain for plane 3 crack accumulated engineering shear strain for plane 1 crack accumulated engineering shear strain for plane 2 crack accumulated engineering shear strain for plane 3 Extra Variable 13: maximum shear utilization to date for plane 1 Extra Variable 14: maximum shear utilization to date for plane 2 Extra Variable 15: maximum shear utilization to date for plane 3 11. Joint planes would generally be defined in the global axis system if they are taken from survey data. However, the material model can also be used to rep- resent masonry, in which case the weak planes represent the cement and lie parallel to the local element axes. *MAT_HYSTERETIC_REINFORCEMENT This is Material Type 203 in LS-DYNA. It is intended as an alternative reinforcement model for layered reinforced concrete shell elements, for use in seismic analysis where the nonlinear hysteretic behaviour of the reinforcement is important. *PART_COM- POSITE or *INTEGRATION_BEAM should be used to define some integration points as a part made of *MAT_HYSTERETIC_REINFORCEMENT, while other integration points have concrete properties using *MAT_CONCRETE_EC2. When using beam elements, ELFORM = 1 is required. Card 1 1 Variable MID Type I 2 RO F 3 YM F 4 PR F 5 6 7 8 SIGY LAMDA SBUCK POWER F F F F Default none 0.0 0.0 0.0 0.0 0.0 SIGY 0.5 Card 2 1 2 3 4 5 6 7 Variable FRACX FRACY LCTEN LCCOMP AOPT EBU DOWNSL Type F F F F F F F Default 0.0 0.0 0.0 0.0 0.0 0.0 0.1 Card 3 1 2 3 4 5 6 7 Variable DBAR FCDOW LCHARD UNITC UNITL Type F F F F F Default 0.0 0.0 0.0 1.0 1.0 Card 4 1 2 3 4 5 6 7 8 Variable EPDAM1 EPDAM2 DRESID Type F F F Default 0.0 0.0 0.0 Additional Card for AOPT ≠ 0. Card 5 Variable 1 XP Type F 2 YP F 3 ZP F 4 A1 F 5 A2 F 6 A3 F Default 0.0 0.0 0.0 0.0 0.0 0.0 7 8 Additional Card for AOPT ≠ 0. Card 6 Variable 1 V1 Type F 2 V2 F 3 V3 F 4 D1 F 5 D2 F 6 D3 F 7 8 BETA F Default 0.0 0.0 0.0 0.0 0.0 0.0 0.0 VARIABLE DESCRIPTION MID Material identification. A unique number has to be chosen. RO YM PR Mass density. Young’s Modulus Poisson’s Ratio SIGY Yield stress VARIABLE DESCRIPTION LAMDA Slenderness ratio SBUCK Initial buckling stress (should be positive) POWER Power law for Bauschinger effect (non-dimensional) FRACX FRACY LCTEN Fraction of reinforcement at this integration point in local 𝑥 direction Fraction of reinforcement at this integration point in local 𝑦 direction Optional curve providing the factor on SIGY versus plastic strain (tension) LCCOMP Optional curve providing the factor on SBUCK versus plastic strain (compression) AOPT Option for local axis alignment – see material type 2 EBU Optional buckling strain (if defined, overrides LAMBDA) DOWNSL Initial down-slope of buckling curve as a fraction of YM (dimensionless) DBAR Reinforcement bar diameter used for dowel action. See remarks. FCDOW Concrete compressive strength used for dowel action. See notes. This field has units of stress LCHARD Characteristic length for dowel action (length units) UNITC UNITL Factor to convert model stress units to MPa, e.g. is model units are Newtons and meters, UNITC = 10−6, [UNITC] = 1/[STRESS]. Factor to convert model length units to millimeters, e.g. if model units are meters, UNITL = 1000, [UNITL] = 1/[LENGTH]. EPDAM1 Accumulated plastic strain at which hysteretic damage begins EPDAM2 Accumulated plastic strain at which hysteretic damage is complete DRESID Residual factor remaining after hysteretic damage XP, YP, ZP Coordinates of point 𝐩 for AOPT = 1 and 4 *MAY_HYSTERETIC_REINFORCEMENT DESCRIPTION A1, A2, A3 Components of vector 𝐚 for AOPT = 2 V1, V2, V3 Components of vector 𝐯 for AOPT = 3 and 4 D1, D2, D3 Components of vector 𝐝 for AOPT = 2 Remarks: Reinforcement is treated as bars, acting independently in the local material 𝑥 and 𝑦 directions. By default, the local material 𝑥-axis is the element 𝑥-axis (parallel to the line from Node 1 to Node 2), but this may be overridden using AOPT or Element Beta angles. The reinforced concrete section should be defined using *INTEGRATION_SHELL, with some integration points being reinforcement (using this material model) and others being concrete (using for example *MAT_CONCRETE_EC2). By default, strains in directions other than the local 𝑥 and 𝑦 are unresisted, so this material model should not be used alone (without concrete). The area fractions of reinforcement in the local 𝑥 and 𝑦 directions at each integration point are given by the area-weighting for the integration point on *INTEGRATION_SHELL times the fractions FRACX and FRACY. The tensile response is elastic perfectly plastic, using yield stress SIGY. Optionally, load curves may be used to describe the stress-strain response in tension (LCTEN) and compression (LCCOMP). Either, neither or both curves may be defined. If present, LCTEN overrides the perfectly-plastic tensile response, and LCCOMP overrides the buckling curve. The tensile and compressive plastic strains are considered independent of each other. Bar buckling may be defined either using the slenderness ratio LAMDA, or by setting the initial buckling strain EBU and down-slope DOWNSL. If neither are defined, the bars simply yield in compression. If both are defined, the buckling behaviour defined by EBU and DOWNSL overrides LAMDA. The slenderness ratio LAMDA determines buckling behaviour and is defined as, Where, 𝑘 depends on end conditions, and 𝐿 = unsupported length of reinforcement bars 𝑘𝐿 , 𝑟 = radius of gyration which for round bars is equal to (bar radius)/√2. It is expected that users will determine LAMDA accounting for the expected crack spacing. The alternative buckling behaviour defined by EBU and DOWNSL is shown below. Compressive stress Yield -DOWNSL * YM -0.005 * YM EBU EBU + 0.01 Compressive strain Reloading after change of load direction follows a Bauschinger-type curve, leading to the hysteresis response shown below: *MAT_HYSTERETIC_REINFORCEMENT ) ( 800 600 400 200 0 -200 -400 -600 -800 -30 -20 -10 0 Strain % 10 20 30 *MAY_HYSTERETIC_REINFORCEMENT Two types of damage accumulation may be modelled. Damage based on ductility (strain) can be modelled using the curves LCTEN and LCCOMP – at high strain, these curves would show reducing stress with increasing strain. Damage based on hysteretic energy accumulation can be modelled using the parameters EPDAM1, EPDAM2 and DRESID. The damage is a function of accumulated plastic strain: for this purpose, plastic strain increments are always treated as positive in both tension and compression, and buckling strain also counts towards the accumulated plastic strain. The material has its full stiffness and strength until the accumulated plastic strain reaches EPDAM1. Between plastic strains EPDAM1 and EPDAM2 the stiffness and strength fall linearly with accumulated plastic strain, reaching a factor DRESID at plastic strain EPDAM2. Dowel Action: The data on Card 3 defines the shear stiffness and strength, and is optional. Shear resistance is assumed to occur by dowel action. The bars bend locally to the crack and crush the concrete. An elastic-perfectly-plastic relation is assumed for all shear components (in-plane and through-thickness). The assumed (smeared) shear modulus and yield stress applicable to the reinforcement bar cross-sectional area are as follows, based on formulae derived from experimental data by El-Ariss, Soroushian, and Dulacska: 𝐺[MPa] = 8.02𝐸0.25𝐹𝑐 0.375𝐿char𝐷𝑏 0.75 where, 𝜏𝑦 = 1.62√𝐹𝑐𝑆𝑦 𝐸 = steel Youngs Modulus in MPa 𝐹𝑐 = 𝑐ompressive strength of concrete in MPa 𝐿char = 𝑐haracteristic length of shear deformation in mm 𝐷𝑏 = bar diameter in mm 𝑆𝑦 = steel yield stress in MPa. The input parameters should be given in model units, e.g. DBAR and LCHAR are in model length units, FCDOW is in model stress units. These will be converted internally using UNITL and UNITC. Output: The output stresses, as for all other LS-DYNA material models, are by default in the global coordinate system. They are scaled by the reinforcement fractions FRACX, FRACY. The plastic strain output is the accumulated plastic strain (increments always treated as positive), and is the greater such value of the two local directions. Extra history variables are available as follows: Total strain in local 𝑥 direction Total strain in local 𝑦 direction Extra variable 1: Reinforcement stress in local 𝑥 direction (not scaled by FRACX) Extra variable 2: Reinforcement stress in local 𝑦 direction (not scaled by FRACY) Extra variable 3: Extra variable 4: Extra variable 5: Accumulated plastic strain in local 𝑥 direction Extra variable 6: Accumulated plastic strain in local 𝑦 direction Extra variable 7: Extra variable 8: Extra variable 9: Shear stress (dowel action) in local 𝑥𝑦 Shear stress (dowel action) in local 𝑥𝑧 Shear stress (dowel action) in local 𝑦𝑧 *MAT_STEEL_EC3 This is Material Type 202. Tables and formulae from Eurocode 3 are used to derive the mechanical properties and their variation with temperature, although these can be overridden by user-defined curves. It is currently available only for Hughes-Liu beam elements. Warning, this material is still under development and should be used with caution. Card 1 1 Variable MID 2 RO Type A8 F 3 E F 4 PR F 5 6 7 8 SIGY F Default none none none none none Card 2 1 2 3 4 5 6 7 8 Variable LC_E LC_PR LC_AL TBL_SS LC_FS Type F F F F F Default none none none none none Card 3 must be included but left blank. Card 3 1 2 3 4 5 6 7 8 Variable Type Default VARIABLE MID DESCRIPTION Material identification. A unique number or label not exceeding 8 characters must be specified. RO Mass density. VARIABLE DESCRIPTION E PR SIGY LC_E LC_PR LC_AL TBL_SS Young’s modulus – a reasonable value must be provided even if LC_E is also input. See notes. Poisson’s ratio. Initial yield stress, 𝜎𝑦0. Optional Loadcurve ID: Young’s Modulus vs Temperature (overrides E and factors from EC3). Optional Loadcurve (overrides PR). ID: Poisson’s Ratio vs Temperature Optional Loadcurve ID: alpha vs temperature (over-rides thermal expansion data from EC3). Optional Table ID containing stress-strain curves at different temperatures (overrides curves from EC3). LC_FS Optional Loadcurve ID: failure strain vs temperature. Remarks: 1. This material model is intended for modelling structural steel in fires. 2. By default, only E, PR and SIGY have to be defined. Eurocode 3 (EC3) Section 3.2 specifies the stress-strain behaviour of carbon steels at tempera- tures between 20C and 1200C. The stress-strain curves given in EC3 are scaled within the material model such that the maximum stress at low tem- peratures is SIGY, see graph below. 3. By default, the Young’s Modulus E will be scaled by a factor which is a function of temperature as specified in EC3. The factor is 1.0 at low temper- ature. 4. By default, the thermal expansion coefficient as a function of temperature will be as specified in EC3 Section 3.4.1.1. 5. LC_E, LC_PR and LC_AL are optional; they should have temperature on the x-axis and the material property on the y-axis, with the points in order of increasing temperature. If present (i.e. non-zero) they over-ride E, PR, and the relationships from EC3. However, a reasonable value for E should al- ways be included, since these values will be used for purposes such as con- tact stiffness calculation. 6. TBL_SS is optional. If present, TBL_SS must be the ID of a *DEFINE_TA- BLE. TBL_SS overrides SIGY and the stress-strain relationships from EC3. The field VALUE on the *DEFINE_TABLE should contain the temperature at which each stress-strain curve is applicable; the temperatures should be in ascending order. The curves that follow the temperature values have (true) plastic strain on the x-axis, (true) yield stress on the y-axis as per other LS- DYNA elasto-plastic material models. As with all instances of *DEFINE TA- BLE, the curves containing the stress-strain data must immediately follow the *DEFINE_TABLE input data and must be in the correct order (i.e. the same order as the temperatures). 7. Temperature can be defined by any of the *LOAD_THERMAL methods. The temperature does not have to start at zero: the initial temperature will be taken as a reference temperature for each element, so non-zero initial temperatures will not cause thermal shock effects. Figure M202-1. *MAT_208 This is Material Type 208 for use with beam elements using ELFORM = 6 (Discrete Beam). The beam elements must have nonzero initial length so that the directions in which tension and compression act can be distinguished. See notes below. Card 1 1 Variable MID 2 RO 3 4 5 6 7 8 KAX KSHR blank blank FPRE TRAMP Type A8 F F F F F Default none none 0.0 0.0 0.0 0.0 Card 2 1 2 3 4 5 6 7 8 Variable LCAX LCSHR FRIC CLEAR DAFAIL DRFAIL DAMAG T0PRE Type Default I 0 I 0 F F F F F F 0.0 0.0 1.E20 1.E20 0.1 0.0 Card 3 must be included but left blank. Card 3 1 2 3 4 5 6 7 8 Variable Type Default VARIABLE MID DESCRIPTION Material identification. A unique number or label not exceeding 8 characters must be specified. RO Mass density. KAX KSHR FPRE DESCRIPTION Axial elastic stiffness (Force/Length units). Shear elastic stiffness (Force/Length units). Preload force. *MAT_BOLT_BEAM TRAMP Time duration during which preload is ramped up. LCAX LCSHR FRIC CLEAR DAFAIL DRFAIL Load curve giving axial load versus plastic displacement (x- axis = displacement (length units), y-axis = force). Load curve ID or table ID giving lateral load versus plastic displacement (x-axis - displacement (length units), y-axis - force). In the table case, each curve in the table represents lateral load versus displacement at a given (current) axial load, i.e. the values in the table are axial forces. Friction coefficient resisting sliding of bolt head/nut (non- dimensional). Radial clearance (gap between bolt shank and the inner diameter of the hole) (length units). Axial tensile displacement at which failure is initiated (length units). Radial displacement at which failure is initiated (excludes clearance). DAMAG Failure is completed at (DAFAIL or DRFAIL)*(1+DAMAG). T0PRE Time at which preload application begins. Remarks: The element represents a bolted joint. The nodes of the beam should be thought of as representing the points at the centers of the holes in the plates that are joined by the bolt. It is expected that SCOOR = 0 on *SECTION_BEAM. This is contrary to the normal rules for non-zero-length discrete beams. The axial direction is initially the line connecting node 1 to node 2. The axial response is tensile-only. Instead of generating a compressive axial load, it is assumed that a gap would develop between the bolt head (or nut) and the surface of the plate. Contact between the bolted surfaces must be modelled separately, e.g. using *CONTACT. Curves LCAX, LCSHR give yield force versus plastic displacement for the axial and shear directions. The force increments are calculated from the elastic stiffnesses, subject to the yield force limits given by the curves. CLEAR allows the bolt to slide in shear, resisted by friction between bolt head/nut and the surfaces of the plates, from the initial position at the center of the hole. CLEAR is the total sliding shear displacement before contact occurs between the bolt shank and the inside surface of the hole. Sliding shear displacement is not included in the displacement used for LCSHR; LCSHR is intended to represent the behaviour after the bolt shank contacts the edge of the hole. Output: beam “axial” or “X” force is the axial force in the beam. “shear-Y” and “shear- Z” are the shear forces. Other output is written to the d3plot and d3thdt files in the places where post- processors expect to find the stress and strain at the first two integration points for integrated beams. Post-Processing data component Actual meaning Int. Pt 1, Axial Stress Change of length Int Pt 1, XY Shear stress Sliding shear displacement in local Y Int Pt 1, ZX Shear stress Sliding shear displacement in local Z Int Pt 1, Plastic strain Resultant shear sliding displacement Int Pt 1, Axial strain Axial plastic displacement Int. Pt 2, Axial Stress Int Pt 2, XY Shear stress Int Pt 2, ZX Shear stress Int Pt 2, Plastic strain Int Pt 2, Axial strain Shear plastic displacement excluding sliding - - - - *MAT_SPR_JLR This is Material Type 211. This material model was written for Self-Piercing Rivets (SPR) connecting aluminium sheets. It intended that each SPR is modelled by a single hexahedral (8-node solid) element, fixed to the sheet either by direct meshing or by tied contact. Pre- and post-processing methods are the same as for solid-element Spotwelds using *MAT_SPOTWELD. On *SECTION_SOLID, set ELFORM = 1. Card 1 1 Variable MID 2 RO Type A8 F 3 E F 4 PR F Default none none none none 5 6 7 8 HELAS TELAS F 0 F 0 Cards 2 and 3 define” Head” end of SPR inputs Card 2 1 2 3 4 5 6 7 8 Variable LCAXH LCSHH LCBMH SFAXH SFSHH SFBMH Type F F F Default none none none Card 3 1 2 3 F 1 4 F 1 5 F 1 6 Variable DFAKH DFSHH RFBMH DMFAXH DMFSHH DMFBMH 7 8 Type F F F F F F Default see notes see notes see notes 0.1 0.1 0.1 Cards 4 and 5 define “Tail” end of SPR inputs Card 4 1 2 3 4 5 6 7 8 Variable LCAXT LCSHT LCBMT SFAXT SFSHT SBFMT Type F F F Default none none none Card 5 1 2 3 F 1 4 F 1 5 F 1 6 Variable DFAXT DFSHT RFBMT DFMAXT DMFSHT DMFBMT 7 8 Type F F F F F F Default see notes see notes see notes 0.1 0.1 0.1 VARIABLE DESCRIPTION MID RO E PR Material identification. A unique number or label not exceeding 8 characters must be specified. Mass density. Young’s modulus, used only for contact stiffness calculation. Poisson’s ratio, used only for contact stiffness calculation. HELAS SPR head end behaviour flag: EQ.0.0: Nonlinear. EQ.1.0: Elastic (Use first two points on load curves). TELAS SPR tail end behaviour flag: EQ.0.0: Nonlinear. EQ.1.0: Elastic (Use first two points on load curves). LCAXH Load curve ID, see *DEFINE_CURVE, giving axial force versus deformation (head). LCSHH *MAT_SPR_JLR DESCRIPTION Load curve ID, see *DEFINE_CURVE, giving shear force versus deformation (head). LCBMH Load curve ID, see *DEFINE_CURVE, giving moment versus rotation (head). SFAXH Scale factor on axial force from curve LCAXH. SFSHH Scale factor on shear force from curve LCSHH. SFBMH Scale factor on bending moment from curve LCBMH. DFAXH Optional displacement to start of softening in axial load (head). DFSHH Optional displacement to start of softening in shear load (head). RFBMH Optional rotation (radians) to start of bending moment softening (head). DMFAXH Scale factor on DFAXH. DMFSHH Scale factor on FFSHH. DMFBMH Scale factor on RFBMH. LCAXT LCSHT LCBMT Load curve ID, see *DEFINE_CURVE, giving axial force versus deformation (tail). Load curve ID, see *DEFINE_CURVE, giving shear force versus deformation (tail). Load curve ID, see *DEFINE_CURVE, giving moment versus rotation (tail). SFAXT Scale factor on axial force from curve LCAXT. SFSHT Scale factor on shear force from curve LCSHT. SFBMT Scale factor on bending moment from curve LCBMT. DFAXT Optional displacement to start of softening in axial load (tail). DFSHT Optional displacement to start of softening in shear load (tail). RFBMT Optional rotation (radians) to start of bending moment softening (tail). VARIABLE DESCRIPTION DMFAXT Scale factor on DFAXT. DMFSHT Scale factor on FFSHT. DMFBMT Scale factor on RFBMT. Remarks: 1. “Head” is the end of the SPR that fully perforates a sheet. “Tail” is the end that is embedded within the thickness of a sheet. 2. E and PR are used only to calculate contact stiffness. They are not used by the material model. 3. Deformation is in length units and is on the x-axis. Force is on the y-axis. Rotation is in radians, on the x-axis. Moment is on the y-axis. 4. All the loadcurves are expected to start at (0,0). “Deformation” means the total deformation including both elastic and plastic components, and similarly for rotation. 5. A “high tide” algorithm is used to determine the deformation or rotation to be used as the x-axis of the loadcurves when looking up the current yield force or moment. The “high tide” is the greatest displacement or rotation that has oc- curred so far during the analysis. 6. The first two points of the curve define the elastic stiffness, which is used for unloading. 7. If HELAS > 0, the remainder of the head loadcurves after the first two points is ignored and no softening or failure occurs. Similarly for TELAS and the tail loadcurves. 8. The sheet planes are defined at the head by the quadrilateral defined by nodes N1-N2-N3-N4 of the solid element; and at the tail by the quadrilateral defined by nodes N5-N6-N7-N8. 9. The tail of the SPR is defined as a point in the tail sheet plane, initially at the centre of the element face. The head of the SPR is initially at the centre of the head sheet plane. Thus the axis of the SPR would typically be coincident with the solid element local z-axis if the solid is a cuboid. It is the user’s responsibil- ity to ensure that each solid element is oriented correctly. 10. During the analysis, the head and tail will always remain in the plane of the sheet, but may move away from the centres of the sheet planes if the shear forces in these planes are sufficient. 11. The SPR axis is defined as the line joining the tail to the head. 12. Axial deformation is defined as change of length of the line between the tail and head of the SPR. This line also defines the direction in which the axial force is applied. 13. Shear deformation is defined as motion of the tail and head points, in the sheet planes. This deformation is not necessarily perpendicular to axial deformation. Shear forces in these planes are controlled by the loadcurves LCSHT and LCSHH. 14. Rotation at the tail is defined as rotation of the tail-to-head line relative to the normal of the tail sheet plane; and for the head, relative to the normal of the head sheet plane. 15. Displacement/rotation to start of softening (DFAXH, DFSHH, etc): if non-zero values are input, these must be within the abcissa values of the relevant curve, such that the curve force/moment value is greater than zero at the defined start of softening. 16. Although ELFORM = 1 is used in the input data, *MAT_SPR_JLR is really a separate unique element formulation. The usual stress/force and hourglass calculations are bypassed, and deformations and nodal forces are calculated by a method unique to *MAT_SPR_JLR; for example, a single *MAT_SPR_JLR element can carry bending loads. 17. *HOURGLASS inputs are irrelevant to *MAT_SPR_JLR. 18. It is essential that the nodes N1 to N4 are fixed to the head sheet (e.g. by direct meshing or tied contact): the element has no stiffness to resist relative motion of nodes N1 to N4 in the plane of the head sheet. Similarly, nodes N5 to N8 must be fixed to the tail sheet. 19. Output to SWFORC file works in the same way as for Spotwelds. Although inside the material model the loadcurves LCSHT and LCSHH control “shear” forces in the sheet planes, in the SWFORC file the quoted shear force is the force normal to the axis of the SPR. 20. Before an element fails, it enters a “softening” regime in which the forces, moments and stiffnesses are ramped down as displacement increases (this avoids sudden shocks when the element is deleted). For example, for axial loading at the head, softening begins when the maximum axial displacement exceeds DFAXH. As the displacement increases beyond that point, the loadcurve will be ignored for that deformation component. The forces, mo- ments and stiffnesses are ramped down linearly with increasing displacement and reach zero at displacement = DFAXH*(1+DMFAXH) when the element is deleted. The softening factor scales all the force and moment components at both head and tail. Thus all the force and moment components are reduced when any one displacement component enters the softening regime. For exam- ple if DFAXT = 3.0mm, and DMFAXT = 0.1, then softening begins when axial displacement of the head reaches 3.0mm and final failure occurs at 3.3mm. 21. If the inputs DFAXT etc are left blank or zero, they will be calculated internally as follows: a) Final failure will occur at the displacement or rotation (DFAIL) at which the loadcurve reaches zero (determined if necessary by extrapolation from the last two points). b) Displacement or rotation at which softening begins is then back- calculated, for example DFAXT = DFAIL/(1+DMGAXT). c) If DMGAXT was left blank or zero, it defaults to 0.1. d) If the loadcurve does not drop to zero, and the final two points have a ze- ro or positive gradient, no failure or softening will be caused by that dis- placement component. 22. Output stresses (in the d3plot and time-history output files) are set to zero. 23. The output variable “displacement ratio” (or rotation ratio for bending), R, is defined as follows. See also the Figure M211-1. a) R = 0 to 1: The maximum force or moment on the input curve has not yet been reached. R is proportional to the maximum force or moment reached so far, with 1.0 being the point of maximum force or moment on the input curve. b) R = 1 to 2: The element has passed the point of maximum force but has not yet entered the softening regime. R rises linearly with displacement (or rotation) from 1.0 when maximum force occurs to 2.0 when softening be- gins. c) R = 2 to 3: Softening is occurring. R rises linearly with displacement from 2.0 at the onset of softening to 3.0 when the element is deleted. Force or moment R=1.0 R=1.0 R=2.0 R=3.0 Linear ramp- down replaces the input loadcurve in the softening regime R=0.0 DF DMF Displacement or Rotation Figure [M211-1]. Output variable “displacement ratio” (or rotation ratio for bending) 24. Displacement (or Rotation) Ratio is calculated separately for axial, shear and bending at the tail and head . The output listed by post-processors as “plastic strain” is actually the maximum displace- ment or rotation ratio of any displacement or rotation component at head or tail. This same variable is also output as “Failure” in the spotweld data in the swforc file (or the swforc section of the binout file). 25. Output extra history variables: 1Failure time (used for SWFORC file) 2(Softening factor used internally to prevent abrupt failure) 3Displacement ratio – axial, head 4Displacement ratio – axial, tail 5Displacement ratio – shear, head 6Displacement ratio – shear, tail 7Rotation ratio – bending, head 8Rotation ratio – bending, tail 9(Used for SWFORC output) 10Shear force in “beam” x-axis 11 Shear force in “beam” y-axis 12Axial force in “beam” z-axis (along “beam”) 13Moment about “beam” x-axis at head 14Moment about “beam” y-axis at head 15Moment about “beam” z-axis at head (torsion – should be zero) 16“Beam” length 17Moment about “beam” x-axis at tail 18Moment about “beam” y-axis at tail 19Moment about “beam” z-axis at tail (torsion – should be zero) 20Isoparametric coordinate of head of “beam” (s) 21Isoparametric coordinate of head of “beam” (t) 22Isoparametric coordinate of tail of “beam” (s) 23Isoparametric coordinate of tail of “beam” (t) 24Timestep 25Plastic displacement, axial, head 26Plastic displacement, axial, tail 27Plastic rotation, head 28Plastic rotation, tail 29Plastic displacement, shear in sheet axes, head 30Plastic displacement, shear in sheet axes, tail 31Beam x-axis (global x component) 32Beam x-axis (global y component) 33Beam x-axis (global z component) 34Shear displacement, local x, head 35Shear displacement, local y, head 36Shear displacement, local x, tail 37Shear displacement, local y, tail 38Total displacement – axial 39Current rotation (radians) – head, local X direction 40Current rotation (radians) – head, local Y direction 41Current rotation (radians) – tail, local X direction 42Current rotation (radians) – tail, local Y direction *MAT_DRY_FABRIC This is Material Type 214. This material model can be used to model high strength woven fabrics, such as Kevlar® 49, with transverse orthotropic behavior for use in structural systems where high energy absorption is required (Bansal et al., Naik et al., Stahlecker et al.). The major applications of the model are for the materials used in propulsion engine containment system, body armor and personal protections. Woven dry fabrics are described in terms of two principal material directions, longitudinal warp and transverse fill yarns. The primary failure mode in these materials is the breaking of either transverse or longitudinal yarn. An equivalent continuum formulation is used and an element is designated as having failed when it reaches some critical value for strain in either directions. A linearized approximation to a typical stress-strain curve is shown in Figure M214-1, and to a typical engineering shear stress-strain curve is shown in the figure corresponding to the GABi field in the variable list. Note that the principal directions are labeled 𝑎 for the warp and 𝑏 for the fill, and the direction 𝑐 is orthogonal to 𝑎 and 𝑏. The material model is available for membrane elements and it is recommended to use a double precision version of LS-DYNA. Card 1 1 Variable MID Type A8 Card 2 1 2 RO F 2 3 EA F 3 4 EB F 4 Variable GBC GCA GAMAB1 GAMAB2 F 2 Type F Card 3 1 Variable AOPT Type F F F 3 XP F 4 YP F 5 6 7 8 GAB1 GAB2 GAB3 F 5 5 ZP F F 6 6 A1 F F 7 7 A2 F 8 8 A3 Variable 1 V1 Type F Card 5 1 2 V2 F 2 3 V3 F 3 4 D1 F 4 5 D2 F 5 6 D3 F 6 *MAT_214 7 8 BETA F 7 8 Variable EACRF EBCRF EACRP EBCRP Type Remarks F 2 Card 6 1 F 2 2 F F 3 4 5 6 7 8 Variable EASF EBSF EUNLF ECOMF EAMAX EBMAX SIGPOST Type Remarks F 2 Card 7 1 F 2 2 F 2 3 F 2 4 F F F 5 6 7 8 Variable CCE PCE CSE PSE DFAC EMAX EAFAIL EBFAIL Type Remarks F 1 F 1 F 1 F 1 F 3 F 4 F 4 F 4 VARIABLE MID DESCRIPTION Material identification. A unique number or label not exceeding 8 characters must be specified. RO Continuum equivalent mass density. SIGPOST E [ A / B ] C E C O M P E[A/B] [ / ] E[A/B]SF These strains values depend on the particular unloading path. Pre-peak linear behavior Post-peak linear behavior Crimp Unloading & Reloading Post-peak non-linear behavior [ / ] [ / Strain ] Failure Strain Figure M214-1. Stress – Strain curve for *MAT_DRY_FABRIC. This curve models the force-response in the longitudinal and transverse directions. VARIABLE DESCRIPTION EA EB GABi / GAMABi GBC GCA AOPT Modulus of elasticity in the longitudinal (warp) direction, which corresponds to the slope of segment AB in Figure M214-1. Modulus of elasticity in the transverse (fill) direction, which corresponds to the slope of segment of AB Figure M214-1. Shear stress-strain behavior is modeled as piecewise linear in three segments. See the figure to the right. The shear moduli GABi correspond to the slope of the ith segment. The start and end points for the segments are specified in the GAMAB[1-2] fields. 𝐺𝑏𝑐, Shear modulus in 𝑏𝑐 direction. 𝐺𝑐𝑎, Shear modulus in 𝑐𝑎 direction. G A B 2 GAB1 Shear Strain Material axes option. See *MAT_OPTIONTROPIC_ELASTIC for a more complete description: EQ.0.0: locally orthotropic with material axes determined by element nodes 1, 2, and 4, as with *DEFINE_COORDI- NATE_NODES, and then rotated about the element normal by an angle BETA. VARIABLE DESCRIPTION EQ.2.0: globally orthotropic with material axes determined by vectors defined below, as with *DEFINE_COORDI- NATE_VECTOR. EQ.3.0: locally orthotropic material axes determined by rotating the material axes about the element normal by an angle, BETA, from a line in the plane of the element defined by the cross product of the vector v with the element nor- mal. LT.0.0: the absolute value of AOPT is a coordinate system ID number (CID on *DEFINE_COORDINATE_NODES, *DEFINE_COORDINATE_SYSTEM or *DEFINE_CO- ORDINATE_VECTOR). Available in R3 version of 971 and later. XP, YP, ZP Components of vector 𝐱. A1, A2, A3 Components of vector 𝐚 for AOPT = 2. V1, V2, V3 Components of vector 𝐯 for AOPT = 3. D1, D2, D3 Components of vector 𝐝 for AOPT = 2. BETA EACRF Material angle in degrees for AOPT = 0 and 3, may be overridden on the element card, see *ELEMENT_SHELL_BETA. Factor for crimp region modulus of elasticity in longitudinal direction : 𝐸𝑎,crimp = 𝐸𝑎,crimpfac𝐸, 𝐸𝑎,crimpfac = EACRF EBCRF Factor for crimp region modulus of elasticity in transverse direction : 𝐸𝑏,crimp = 𝐸𝑏,crimpfac𝐸, 𝐸𝑏,crimpfac = EBCRF EACRP Crimp strain in longitudinal direction : 𝜀𝑎,crimp EBCRP Crimp strain in transverse direction : 𝜀𝑏,crimp EASF *MAT_DRY_FABRIC DESCRIPTION Factor for post-peak region modulus of elasticity in longitudinal direction : 𝐸𝑎,soft = 𝐸𝑎,softfac𝐸, 𝐸𝑎,softfac = EASF EBSF Factor for post-peak region modulus of elasticity in transverse direction : 𝐸𝑏,soft = 𝐸𝑏,softfac𝐸, 𝐸𝑏,softfac = EBSF EUNLF Factor for unloading modulus of elasticity : 𝐸unload = 𝐸unloadfac𝐸, 𝐸unloadfac = EUNLF ECOMPF Factor for compression zone modulus of elasticity : 𝐸comp = 𝐸compfac𝐸, 𝐸compfac = ECOMPF EAMAX Strain at peak stress in longitudinal direction : 𝜀𝑎,max EBMAX Strain at peak stress in transverse direction : 𝜀𝑏,𝑚𝑎𝑥 SIGPOST Stress value in post-peak region at which nonlinear behavior begins : 𝜎post CCE PCE CSE PSE Strain rate parameter 𝐶, Cowper-Symonds factor for modulus. If zero, rate effects are not considered. Strain rate parameter 𝑃, Cowper-Symonds factor for modulus. If zero, rate effects are not considered. Strain rate parameter 𝐶, Cowper-Symonds factor for stress to peak / failure. If zero, rate effects are not considered. Strain rate parameter 𝑃, Cowper-Symonds factor for stress to peak / failure. If zero, rate effects are not considered. DFAC Damage factor: 𝑑fac VARIABLE DESCRIPTION EMAX Erosion strain of element: 𝜀max EAFAIL Erosion strain in longitudinal direction : 𝜀𝑎,fail EBFAIL Erosion strain in transverse direction : 𝜀𝑏,fail Remarks: 1. Strain rate effects are accounted for using a Cowper-Symonds model which scales the stress according to the strain rate: 𝛔adj = 𝛔 (1 + ) . 𝜀̇ In the above equation 𝛔 is the quasi-static stress, 𝛔adj is the adjusted stress ac- counting for strain rate 𝜀̇, 𝐶 (CCE) and 𝑃 (PCE) are the Cowper-Symonds factors and have to be determined experimentally for each material. The model captures the non-linear strain rate effects in many materials. With its less than unity exponent, 1/𝑝 , this model captures the rapid increase in material properties at low strain rate, while increasing less rapidly at very high strain rates. Because stress is a function of strain rate the elastic stiffness also is: 𝐄adj = 𝐄 (1 + ) 𝜀̇ where 𝐄adj is the adjusted elastic stiffness. Additionally, the strains to peak and strains to failure are assumed to follow a Cowper-Symonds model with, possibly different, constants 𝜀adj = ε (1 + 𝑃𝑠 ) 𝜀̇ 𝐶𝑠 where, 𝜀adj is the adjusted effective strain to peak stress or strain to failure, and 𝐶𝑠 and 𝑃𝑠 are CSE and PSE respectively. 2. When strained beyond the peak stress, the stress decreases linearly until it attains a value equal to SIGPOST, at which point the stress-strain relation be- comes nonlinear. In the non-linear region the stress is given by 𝜎 = 𝜎post ⎢⎡1 − ( ⎣ 𝜀 − 𝜀[𝑎/𝑏],post 𝜀[𝑎/𝑏],fail − 𝜀[𝑎/𝑏],post ) 𝑑fac ⎥⎤ ⎦ where 𝜎post and 𝜀post are, respectively, the stress and strain demarcating the onset of nonlinear behavior. The value of SIGPOST is the same in both the transverse and longitudinal directions, whereas 𝜀a,post and 𝜀b,post depend on direction and are derived internally from EASF, EBSF, and SIGPOST. The fail- ure strain, 𝜀[𝑎/𝑏],fail, specifies the onset of failure and differs in the longitudinal and transverse directions. Lastly the exponent, 𝑑fac, determines the shape of nonlinear stress-strain curve between 𝜀post and 𝜀[𝑎 𝑏⁄ ],fail. 3. The element is eroded if either (a) or (b) is satisfied: a) 𝜀𝑎 > 𝜀𝑎,fail and 𝜀𝑏 > 𝜀𝑏,fail b) 𝜀𝑎 > 𝜀max and 𝜀𝑏 > 𝜀max. *MAT_215 This is Material Type 215. A micromechanical material that distinguishes between a fiber/inclusion and a matrix material, developed by 4a engineering GmbH. It is available for the explicit code for shell, thick shell and solid elements. Useful hints and input example can be found in [1]. More theory and application notes will be provided soon in [2]. The material is intended for anisotropic composite materials, especially for short (SFRT) and long fiber thermoplastics (LFRT). The matrix behavior is described by an isotropic elasto-viscoplastic von Mises model. The fiber/inclusion behavior is transversal isotropic elastic. This also allows to use this material model for classical endless fiber composites. The inelastic homogenization for describing the composite deformation behavior is based on: •Mori Tanaka Meanfield Theory [3,4] •ellipsoidal inclusions using Eshelby´s solution [5,6] •orientation averaging [7] •a linear fitted closure approximation to determine the 4th order fiber orientation tensor out of the user provided 2nd order fiber orientation tensor. The core functionality to calculate the thermo-elastic composite properties can be also found in the software product 4a micromec [8]. Failure/Damage of the composite can be currently considered by •a ductile damage initiation and evolution model for the matrix (DIEM) •fiber failure may be considered with a maximum stress criterion. More details on the material characterization can be found in [9] and [10]. The (fiber) orientation can be defined either for the whole material using CARD 2 and 3 or elementwise using *ELEMENT_(T)SHELL_BETA or *ELEMENT_SOLID_ORTHO. The mechanical properties of SFRT and LFRT in injection molded parts are highly influenced through the manufacturing process. By mapping the fiber orientation from the process simulation to the structural analysis the local anisotropy can be considered [11,12]. The fiber orientation, length and volume fraction can therefore as well be defined for each integration point by using *INITIAL_STRESS_(T)SHELL(SOLID) [2]. Details on the history variables that can be initialized (Extravars. 9-18) can be found in the output section. *MAT_4A_MICROMEC Card 1 1 2 3 4 5 6 7 8 Variable MID MMOPT BUPD FAILM FAILF NUMINT Type A8 F F F F F Default none 0.0 0.01 0.0 0.0 1.0 Parameter for fiber orientation (may be overwritten by *INITIAL_STRESS_SHELL/SOLID) Card 2 1 2 Variable AOPT MACF Type F Default 0.0 Card 3 Variable 1 V1 Type F F 0 2 V2 F 3 XP F 4 YP F 5 ZP F 6 A1 F 7 A2 F 8 A3 F 0.0 0.0 0.0 0.0 0.0 0.0 3 V3 F 4 D1 F 5 D2 F 6 D3 F 7 8 BETA F Default 0.0 0.0 0.0 0.0 0.0 0.0 0.0 1 2 Variable FVF Type F 3 FL F 4 FD F *MAT_215 5 6 7 8 A11 A22 F F Default 0.0 0.0 1.0 1.0 0.0 Parameter for fiber/inclusion material Card 5 1 Variable ROF Type F 2 EL F 3 ET F 4 5 6 7 8 GLT PRTL PRTT F F F Default 0.0 0.0 0.0 0.0 0.0 0.0 2 3 4 5 6 7 8 Card 6 Variable 1 XT Type F Default 0.0 Parameter for matrix material Card 7 1 Variable ROM Type F 2 E F 3 PR F Default 0.0 0.0 0.0 SLIMXT NCYRED F F 0.0 10 4 5 6 7 Card 8 1 2 3 4 5 Variable SIGYT ETANT Type F F EPS0 F 6 C F 7 8 Default 0.0 0.0 0.0 0.0 Card 9 1 2 3 4 5 6 7 8 Variable LCIDT LCDI UPF Type Default F 0 VARIABLE MID F 0 F 0.0 DESCRIPTION Material identification. A unique number or label not exceeding 8 characters must be specified. MMOPT Option to define micromechanical material behavior EQ.0.0: elastic EQ.1.0: elastic-plastic BUPD Tolerance for update of Strain-Concentration Tensor VARIABLE FAILM DESCRIPTION Opion for matrix failure – ductile DIEM-Model. based on stress triaxiality and a linear damage evolution (DETYP.EQ.0) type) LT.0: |FAILM| Effective plastic matrix strain at failure. When the matrix plastic strain reaches this value, the element is deleted from the calculation. EQ.0: only visualization (triaxiality of matrix stresses) EQ.1: active DIEM (triaxiality of matrix stresses) EQ.10: only visualization (triaxiality of composite stresses) EQ.11: active DIEM (triaxiality of composite stresses) FAILF Option for fiber failure EQ.0: only visualization (equivalent fiber stresses) EQ.1: active (equivalent fiber stresses) NUMINT Number of failed integration points prior to element deletion. LT.0.0: Only for shells. |NUMINT| is the percentage of integration points which must exceed the failure criterion before element fails. For shell formulations with 4 inte- gration points per layer, the layer is considered failed if any of the integration points in the layer fails. Parameter for fiber orientation AOPT See *MAT_002 (fiber orientation information may be overwritten using *INITIAL_STRESS_(T)SHELL/SOLID) MACF Material axes change flag for solid elements: EQ.1: No change, default, EQ.2: switch material axes a and b, EQ.3: switch material axes a and c, EQ.4: switch material axes b and c. XP, YP, ZP Define coordinates of point p for AOPT = 1 and 4. A1, A2, A3 Define components of vector a for AOPT = 2. *MAT_4A_MICROMEC DESCRIPTION V1, V2, V3 Define components of vector v for AOPT = 3 and 4. D1, D2, D3 Define components of vector d for AOPT = 2. BETA Material angle in degrees for AOPT = 3, may be overwritten on the element card, see *ELEMENT_(T)SHELL_BETA or *ELEMENT_SOLID_ORTHO. FVF Fiber-Volume-Fraction GT.0: Fiber-Volume-Fraction LT.0: |FVF| Fiber-Mass-Fraction FL FD A11 A22 Fiber length - if FD = 1 then FL = aspect ratio (may be overwritten by *INITIAL_STRESS_(T)SHELL/SOLID) Fiber diameter (may be overwritten by *INITIAL_STRESS_(T)SHELL/SOLID) Value of first principal fiber orientation (may be overwritten by *INITIAL_STRESS_(T)SHELL/SOLID). Value of second principal fiber orientation (may be overwritten by *INITIAL_STRESS_(T)SHELL/SOLID). Parameter for fiber/inclusion material ROF Mass density of fiber EL ET GLT PRTL PRTT XT EL, Young’s modulus of fiber – longitudinal direction. ET, Young’s modulus of fiber – transverse direction. GLT, Shear modulus LT TL, Poisson’s ratio TL TT, Poisson’s ratio TT Fiber tensile strength – longitudinal direction. SLIMXT Factor to determine the minimum stress limit in the fiber after stress maximum (fiber tension) NCYRED Number of cycles for stress reduction from maximum to minimum (fiber tension) Parameter for matrix material ROM Mass density of matrix. E PR SIGYT ETANT EPS0 C LCIDT Young’s modulus of matrix. Poisson’s ratio of matrix. Yield stress of matrix in tension Tangent modulus of matrix in tension, ignore if (LCST.GT.0.) is defined. Quasi-static threshold strain rate (Johnson-Cook model) for bi- linear hardening Johnson-Cook constant for bi-linear hardening Load curve ID or Table ID for defining effective stress versus effective plastic strain in tension of matrix material (Table to include strain-rate effects, viscoplastic formulation) LCDI Damage initiation parameter (ductile) shells: Load curve ID representing plastic strain at onset of damage as function of stress triaxiality. or Table ID representing plastic strain at onset of damage as function of stress triaxiality and plastic strain rate. solids: Load curve ID representing plastic strain at onset of damage as function of stress triaxiality. or Table ID representing plastic strain at onset of damage as function of stress triaxiality and lode angle. or Table3D ID representing plastic strain at onset of damage as function of stress triaxiality, lode angle and plastic strain rate. UPF Damage evolution parameter 𝑝 GT.0.0: plastic displacement at failure, 𝑢𝑓 LT.0.0: |UPF| is a table ID for 𝑢𝑓 𝑝 as a function of triaxiality and damage Output: “Plastic Strain” is the equivalent plastic strain in the matrix. Extra history variables may be requested for (t)shell (NEIPS) and solid (NEIPH) elements on *DATABASE_EXTENT_BINARY. Extra history variables 1-8 are intended for post processing, 9-18 for initialization with *INITIAL_STRESS_(T)SHELL/SOLID. They have the following meaning: Extravar. DESCRIPTION 1 2 3 4 5 6 7 8 effs - equivalent plastic strain rate of matrix eta - triaxiality of matrix ... = − q xi - lode parameter of matrix ... = − 27∙J3 2∙q dM - Damage initiation d of matrix (Ductile Criteria) DM - Damage evolution D of matrix RFF - Fiber reserve factor DF- Fiber damage variable Currently unused Extravar. DESCRIPTION 9 10 11 12 13 14 15 16 A11 - fiber orientation first principal value A22 - fiber orientation first second value q1/q11 q2/q12 -/q13 -/q31 -/q32 -/q33 17 18 FVF- Fiber-Volume-Fraction FL- Fiber length References: [1] Reithofer, P., et. al, *MAT_4A_MICROMEC – micro mechanic based material model, 14th German LS-DYNA Conference (2016), Bamberg [2] Reithofer, P., et. al, *MAT_4A_MICROMEC – Theory and application notes, 11th European LS- DYNA Conference (2017), Salzburg [3] Mori, T., Tanaka, K., Average Stress in Matrix and Average elastic Energy of Materials with misfitting Inclusions, Acta Metallurgica, Vol.21, pp.571-574, (1973). [4] Tucker Ch. L. III, Liang Erwin: Stiffness Predictions for Unidirectional Short-Fibre Composites: Review and Evaluation, Composites Science and Technology, 59, (1999) [5] Maewal A., Dandekar D.P.: Effective Thermoelastic Properties of Short-Fibre Composites, Acta Mechanica, 66, (1987) [6] Eshelby, J. D., The determination of the elastic field of an ellipsoidal inclusion, and related problems, Proceedings of the Royal Society, London, Vol.A, No241, pp.376-396, (1957). [7] Mlekusch, B., Kurzfaserverstärkte Thermoplaste, Dissertation, Montanuniversität Leoben (1997) [8] http://micromec.4a.co.at [9] Reithofer, P. et. al: Material characterization of composites using micro mechanic models as key enabler, NAFEMS DACH, Bamberg 2016 [10] http://impetus.4a.co.at [11] Reithofer, P. et. al: Short and long fiber reinforced thermoplastics material models in LS-DYNA, 10th European LS-DYNA Conference, Würzburg 2015 [12] http://fibermap.4a.co.at *MAT_ELASTIC_PHASE_CHANGE This is Material Type 216, a generalization of Material Type 1, for which material properties change on an element-by-element basis upon crossing a plane in space. This is an isotropic hypoelastic material and is available only for shell element types. 5 6 7 8 5 6 7 8 Phase 1 Properties. Card 1 1 2 Variable MID RO1 Type A8 F 3 E1 F 4 PR1 F Default none none none 0.0 Phase 2 Properties. Card 1 1 2 Variable Type RO2 F 3 E2 F 4 PR2 F Default none none 0.0 Transformation Plane Card. Card 2 Variable 1 X1 Type F 2 Y1 F 3 Z1 F 4 X2 F 5 Y2 F 6 Z2 F 7 8 THKFAC F Default none none none none none none 1.0 VARIABLE DESCRIPTION MID ROi Ei PRi Material identification. A unique number or label not exceeding 8 characters must be specified. Mass density for phase i. Young’s modulus for phase i. Poisson’s ratio for phase i. X1, Y1, Z1 Coordinates of a point on the phase transition plane. Coordinates of a point that defines the exterior normal with the first point. Scale factor applied to the shell thickness after the phase transformation. X2, Y2, Z2 THKFAC Phases: The material properties for each element are initialized using the data for the first phase. After the center of the element passes through the transition plane defined by the two points, the material properties are irreversibly changed to the second phase. The plane is defined by two points. The first point, defined by the coordinates X1, Y1, and Z1, lies on the plane. The second point, defined by the coordinates X2, Y2, and Z2, define the exterior normal as a unit vector in the direction from the first point to the second point. Remarks: This hypoelastic material model may not be stable for finite (large) strains. If large strains are expected, a hyperelastic material model, e.g., *MAT_002 or *MAT_217, would be more appropriate. *MAT_OPTIONTROPIC_ELASTIC_PHASE_CHANGE This is Material Type 217 a generalization of Material Type 2 for which material properties change on an element-by-element basis upon crossing a plane in space. This material is valid only for shells. The stress update is incremental and the elastic constants are formulated in terms of Cauchy stress and true strain. Available options include: ORTHO ANISO such that the keyword cards appear: *MAT_ORTHOTROPIC_ELASTIC_PHASE_CHANGE or MAT_217 (9 cards follow) *MAT_ANISOTROPIC_ELASTIC_PHASE_CHANGE or MAT_217_ANIS (11 cards follow) Orthotropic Card 1 (phase 1). Card 1 for ORTHO keyword option for phase 1. Card 1 1 2 Variable MID RO1 Type A8 F 3 EA F 4 EB F 5 EC F 6 7 8 PRBA PRCA PRCB F F F Orthotropic Card 2 (phase 1). Card 2 for ORTHO keyword option for phase 1. Card 2 1 2 3 4 Variable GAB GBC GCA AOPT1 Type F F F F 5 G F 6 7 8 SIGF Anisotropic Card 1 (phase 1). Card 1 for ANISO keyword option for phase 1. Card 1 1 2 3 4 5 6 7 8 Variable MID RO2 C111 C121 C221 C131 C231 C331 Type A8 F F F F F F F Anisotropic Card 2 (phase 1). Card 2 for ANISO keyword option for phase 1. Card 2 1 2 3 4 5 6 7 8 Variable C141 C241 C341 C441 C151 C251 C351 C451 Type F F F F F F F F Anisotropic Card 3 (phase 1). Card 3 for ANISO keyword option for phase 1. Card 3 1 2 3 4 5 6 7 8 Variable C551 C161 C261 C361 C461 C561 C661 AOPT1 Type F F F F F F F F Local Coordinate System Card 1 (phase 1). Required for all keyword options Card 4 1 2 3 4 5 6 7 8 Variable XP1 YP1 ZP1 A11 A21 A31 MACF IHIS Type F F F F F F I F Local Coordinate System Card 2 (phase 1). Required for all keyword options Card 5 1 2 3 4 5 6 7 8 Variable V11 V21 V31 D11 D21 D31 BETA1 REF Type F F F F F F F Orthotropic Card 3 (phase 2). Card 1 for ORTHO keyword option phase 2. Card 6 1 2 3 4 5 6 7 8 Variable Type EA2 EB2 EC2 PRBA2 PRCA2 PRCB2 F F F F F F Orthotropic Card 4 (phase 2). Card 2 for ORTHO keyword option phase 2. Card 7 1 2 3 4 5 6 7 8 Variable GAB2 GBC2 GCA2 Type F F F Anisotropic Card 4 (phase 2). Card 1 for ANISO keyword option for phase 2. Card 6 1 2 3 4 5 6 7 8 Variable Type C112 C122 C222 C132 C232 C332 F F F F F F Anisotropic Card 5 (phase 2). Card 2 for ANISO keyword option for phase 2. Card 7 1 2 3 4 5 6 7 8 Variable C142 C242 C342 C442 C152 C252 C352 C452 Type F F F F F F F Anisotropic Card 6 (phase 2). Card 3 for ANISO keyword option for phase 2. Card 8 1 2 3 4 5 6 7 8 Variable C552 C162 C262 C362 C462 C562 C662 Type F F F F F F F Local Coordinate System Card 1 (phase 2). Required for all keyword options Card 9 1 2 3 4 5 6 7 8 Variable XP2 YP2 ZP2 A12 A22 A32 MACF2 Type F F F F F F I Local Coordinate System Card 2 (phase 2). Required for all keyword options Card 10 1 2 3 4 5 6 7 8 Variable V12 V22 V32 D12 D22 D32 BETA2 Type F F F F F F F Definition of transformation plane Card. Card 11 Variable 1 X1 Type F 2 Y1 F 3 Z1 F 4 X2 F 5 Y2 F 6 Z2 F 7 8 THKFAC F Default none none none none none none 1.0 VARIABLE MID DESCRIPTION Material identification. A unique number or label not exceeding 8 characters must be specified. ROi Mass density for phase i. Define for the ORTHO option only: EAi EBi ECi PRBAi PRCAi PRCBi GABi GBCi GCAi 𝐸𝑎, Young’s modulus in 𝑎-direction for phase i. 𝐸𝑏, Young’s modulus in 𝑏-direction for phase i. 𝐸𝑐, Young’s modulus in 𝑐-direction phase i (nonzero value required but not used for shells). 𝜈𝑏𝑎, Poisson’s ratio in the 𝑏𝑎 direction for phase i. 𝜈𝑐𝑎, Poisson’s ratio in the ca direction for phase i. 𝜈𝑐𝑏, Poisson’s ratio in the 𝑐𝑏 direction for phase i. 𝐺𝑎𝑏, shear modulus in the ab direction for phase i. 𝐺𝑏𝑐, shear modulus in the 𝑏𝑐 direction for phase i. 𝐺𝑐𝑎, shear modulus in the 𝑐𝑎 direction for phase i. Due to symmetry define the upper triangular Cij’s for the ANISO option only: C11i C12i ⋮ C66i The 1,1 term in the 6 × 6 anisotropic constitutive matrix for phase i. Note that 1 corresponds to the 𝑎 material direction The 1,2 term in the 6 × 6 anisotropic constitutive matrix for phase i. Note that 2 corresponds to the 𝑏 material direction ⋮ The 6,6 term in the 6 × 6 anisotropic constitutive matrix for phase i. Define AOPT for both options: AOPTi Material axes option for phase i, see Figure M2-1. EQ.0.0: locally orthotropic with material axes determined by element nodes as shown in part (a) of Figure M2-1. The a-direction is from node 1 to node 2 of the element. The b-direction is orthogonal to the a-direction and is in the plane formed by nodes 1, 2, and 4. When this option is used in two-dimensional planar and axisym- metric analysis, it is critical that the nodes in the ele- ment definition be numbered counterclockwise for this option to work correctly. EQ.1.0: locally orthotropic with material axes determined by a point in space and the global location of the element center; this is the 𝐚-direction. This option is for solid elements only. EQ.2.0: globally orthotropic with material axes determined by vectors defined below, as with *DEFINE_COORDI- NATE_VECTOR. EQ.3.0: locally orthotropic material axes determined by rotating the material axes about the element normal by an angle, BETA, from a line in the plane of the element defined by the cross product of the vector 𝐯 with the element normal. The plane of a solid element is the midsurface between the inner surface and outer surface defined by the first four nodes and the last four nodes of the connectivity of the element, respectively. EQ.4.0: locally orthotropic in cylindrical coordinate system with the material axes determined by a vector 𝐯, and an originating point, 𝐏, which define the centerline ax- is. This option is for solid elements only. LT.0.0: the absolute value of AOPT is a coordinate system ID number (CID on *DEFINE_COORDINATE_NODES, *DEFINE_COORDINATE_SYSTEM or *DEFINE_CO- ORDINATE_VECTOR). Available in R3 version of 971 and later. G Shear modulus for frequency independent damping. Frequency independent damping is based of a spring and slider in series. The critical stress for the slider mechanism is SIGF defined below. For the best results, the value of G should be 250-1000 times greater than SIGF. This option applies only to solid elements. SIGF Limit stress for frequency independent, frictional, damping. XPi, YPi, ZPi Define coordinates of the ith phase’s point 𝐩 for AOPT = 1 and 4. A1i, A2i, A3i Define components of the ith phase’s vector 𝐚 for AOPT = 2. MACFi Material axes change flag for brick elements in phase i: EQ.1: No change, default, EQ.2: switch material axes 𝑎 and 𝑏, EQ.3: switch material axes 𝑎 and 𝑐, EQ.4: switch material axes 𝑏 and 𝑐. IHIS Flag for anisotropic stiffness terms initialization (for solid elements only). EQ.0: C11, C12, … from Cards 1, 2, and 3 are used. EQ.1: C11, C12, … are initialized by *INITIAL_STRESS_SOL- ID’s history data. V1i, V2i, V3i Define components of the ith phase’s vector 𝐯 for AOPT = 3 and 4. D1i, D2i, D3i Define components of the ith phase’s vector 𝐝 for AOPT = 2. BETAi REFi Material angle of ith phase in degrees for AOPT = 3, may be overridden on the element card, see *ELEMENT_SHELL_BETA or *ELEMENT_SOLID_ORTHO. Use reference geometry to initialize the stress tensor for the ith phase. The reference geometry is defined by the keyword: *INI- TIAL_FOAM_REFERENCE_GEOMETRY . EQ.0.0: off, EQ.1.0: on. X1, Y1, Z1 Coordinates of a point on the phase transition page. Coordinates of a point that defines the exterior normal with the first point. Scale factor applied to the shell thickness after the phase transformation. X2, Y2, Z2 THKFAC Phases: The material properties for each element are initialized using the data for the first phase. After the center of the element passes through the transition plane defined by the two points, the material properties are irreversibly changed to the second phase. The plane is defined by two points. The first point, defined by the coordinates X1, Y1, and Z1, lies on the plane. The second point, defined by the coordinates X2, Y2, and Z2, define the exterior normal as a unit vector in the direction from the first point to the second point. Material Formulation: The material law that relates stresses to strains is defined as: 𝐂 = 𝐓T𝐂𝐿𝐓 where 𝐓 is a transformation matrix, and 𝐂𝐿 is the constitutive matrix defined in terms of the material constants of the orthogonal material axes, {𝐚, 𝐛, 𝐜}. The inverse of 𝐂𝐿for the orthotropic case is defined as: −1 = 𝐂𝐿 𝐸𝑎 𝜐𝑎𝑏 𝐸𝑎 𝜐𝑎𝑐 𝐸𝑎 − − − − 𝜐𝑏𝑎 𝐸𝑏 𝐸𝑏 𝜐𝑏𝑐 𝐸𝑏 − − 𝜐𝑐𝑎 𝐸𝑐 𝜐𝑐𝑏 𝐸𝑐 𝐸𝑐 ⎡ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎣ 𝐺𝑎𝑏 𝐺𝑏𝑐 ⎤ ⎥ ⎥ ⎥ ⎥ ⎥ ⎥ ⎥ ⎥ ⎥ ⎥ ⎥ ⎥ ⎥ ⎥ ⎥ ⎥ 𝐺𝑐𝑎⎦ Where, 𝜐𝑎𝑏 𝐸𝑎 = 𝜐𝑏𝑎 𝐸𝑏 , 𝜐𝑐𝑎 𝐸𝑐 = 𝜐𝑎𝑐 𝐸𝑎 , 𝜐𝑐𝑏 𝐸𝑐 = 𝜐𝑏𝑐 𝐸𝑏 . The frequency independent damping is obtained by having a spring and slider in series as shown in the following sketch: friction This option applies only to orthotropic solid elements and affects only the deviatoric stresses. The procedure for describing the principle material directions is explained for solid and shell elements for this material model and other anisotropic materials. We will call the material direction the {𝐚, 𝐛, 𝐜} coordinate system. The AOPT options illustrated in Figure M2-1 can define the {𝐚, 𝐛, 𝐜} system for all elements of the parts that use the material, but this is not the final material direction. There {𝐚, 𝐛, 𝐜} system defined by the AOPT options may be offset by a final rotation about the 𝐜-axis. The offset angle we call BETA. For solid elements, the BETA angle is specified in one of two ways. When using AOPT = 3, the BETA parameter defines the offset angle for all elements that use the material. The BETA parameter has no meaning for the other AOPT options. Alternatively, a BETA angle can be defined for individual solid elements as described in remark 5 for *ELEMENT_SOLID_ORTHO. The beta angle by the ORTHO option is available for all values of AOPT, and it overrides the BETA angle on the *MAT card for AOPT = 3. The directions determined by the material AOPT options may be overridden for individual elements as described in remark 3 for *ELEMENT_SOLID_ORTHO. However, be aware that for materials with AOPT = 3, the final {𝐚, 𝐛, 𝐜} system will be the system defined on the element card rotated about 𝐜-axis by the BETA angle specified on the *MAT card. There are two fundamental differences between shell and solid element orthotropic materials. First, the 𝐜-direction is always normal to a shell element such that the 𝐚- direction and 𝐛-directions are within the plane of the element. Second, for some anisotropic materials, shell elements may have unique fiber directions within each layer through the thickness of the element so that a layered composite can be modeled with a single element. When AOPT = 0 is used in two-dimensional planar and axisymmetric analysis, it is critical that the nodes in the element definition be numbered counterclockwise for this option to work correctly. Because shell elements have their 𝐜-axes defined by the element normal, AOPT = 1 and AOPT = 4 are not available for shells. Also, AOPT = 2 requires only the vector 𝐚 be defined since 𝐝 is not used. The shell procedure projects the inputted 𝐚-direction onto each element surface. Similar to solid elements, the {𝐚, 𝐛, 𝐜} coordinate system determined by AOPT is then modified by a rotation about the 𝐜-axis which we will call 𝜙. For those materials that allow a unique rotation angle for each integration point through the element thickness, the rotation angle is calculated by 𝜙𝑖 = 𝛽 + 𝛽𝑖 where 𝛽 is a rotation for the element, and 𝛽𝑖 is the rotation for the i’th layer of the element. The 𝛽 angle can be input using the BETA parameter on the *MAT data, or will be overridden for individual elements if the BETA keyword option for *ELEMENT_- SHELL is used. The 𝛽𝑖 angles are input using the ICOMP = 1 option of *SECTION_- SHELL or with *PART_COMPOSITE. If 𝛽 or 𝛽𝑖 is omitted, they are assumed to be zero. All anisotropic shell materials have the BETA option on the *MAT card available for both AOPT = 0 and AOPT = 3, except for materials 91 and 92 which have it available for all values of AOPT, 0, 2, and 3. All anisotropic shell materials allow an angle for each integration point through the thickness, 𝛽𝑖, except for materials 2, 86, 91, 92, 117, 130, 170, 172, and 194. This discussion of material direction angles in shell elements also applies to thick shell elements which allow modeling of layered composites using *INTEGRATION_SHELL or *PART_COMPOSITE_TSHELL. *MAT_MOONEY-RIVLIN_PHASE_CHANGE This is Material Type 218, a generalization of Material Type 27, for which material properties change on an element-by-element basis upon crossing a plane in space. Phase 1 Card 1. Card 1 1 2 3 Variable MID RO1 PR1 Type A8 F F 4 A1 F 5 B1 F 6 REF F 7 8 Phase 1 Card 2. Card 2 1 2 3 4 5 6 7 8 Variable SGL1 SW1 ST1 LCID1 Type F F F F Phase 2 Card 1. Card 3 1 2 3 Variable RO2 PR2 Type F F 4 A2 F 5 B2 F 6 7 8 Phase 2 Card 2. Card 4 1 2 3 4 5 6 7 8 Variable SGL2 SW2 ST2 LCID2 Type F F F Transformation Plane Card. Card 5 Variable 1 X1 Type F 2 Y1 F 3 Z1 F 4 X2 F 5 Y2 F 6 Z2 F 7 8 THKFAC F Default none none none none none none 1.0 VARIABLE DESCRIPTION MID ROi PRi Ai Bi REF Material identification. A unique number or label not exceeding 8 characters must be specified. Mass density for phase i. Poisson’s ratio (value between 0.49 and 0.5 is recommended, smaller values may not work) where i indicates the phase. Constant for the ith phase, see literature and equations defined below. Constant for the ith phase, see literature and equations defined below. Use reference geometry to initialize the stress tensor. The reference geometry is defined by the keyword:*INITIAL_FOAM_- REFERENCE_GEOMETRY . EQ.0.0: off, EQ.1.0: on. gauge length Force AA Δ gauge length Section AA thickness width Figure M218-1. Uniaxial specimen for experimental data If A = B = 0.0, then a least square fit is computed from tabulated uniaxial data via a load curve. The following information should be defined: VARIABLE DESCRIPTION SGLi SWi STi LCIDi Specimen gauge length 𝑙0 for the ith phase, see Figure M218-1. Specimen width for the ith phase, see Figure M218-1. Specimen thickness for the ith phase, see Figure M218-1. Curve ID for the ith phase, see *DEFINE_CURVE, giving the force versus actual change Δ𝐿 in the gauge length. See also Figure M218-2 for an alternative definition. X1, Y1, Z1 Coordinates of a point on the phase transition plane. X2, Y2, Z2 THKFAC Coordinates of a point that defines the exterior normal with the first point. Scale factor applied to the shell thickness after the phase transformation. Phases: The material properties for each element are initialized using the data for the first phase. After the center of the element passes through the transition plane defined by the two points, the material properties are irreversibly changed to the second phase. The plane is defined by two points. The first point, defined by the coordinates X1, Y1, and Z1, lies on the plane. The second point, defined by the coordinates X2, Y2, and Z2, define the exterior normal as a unit vector in the direction from the first point to the second point. Material Formulation: The strain energy density function is defined as: 𝑊 = 𝐴(𝐼 − 3) + 𝐵(𝐼𝐼 − 3) + 𝐶(𝐼𝐼𝐼−2 − 1) + 𝐷(𝐼𝐼𝐼 − 1)2 where 𝐶 = 0.5 𝐴 + 𝐵 𝐷 = 𝐴(5𝜐 − 2) + 𝐵(11𝜐 − 5) 2(1 − 2𝜐) 𝜈 = Poisson’s ratio 2(𝐴 + 𝐵) = shear modulus of linear elasticity 𝐼, 𝐼𝐼, 𝐼𝐼𝐼 = invariants of right Cauchy-Green Tensor C. The load curve definition that provides the uniaxial data should give the change in gauge length, Δ𝐿, versus the corresponding force. In compression both the force and the change in gauge length must be specified as negative values. In tension the force and change in gauge length should be input as positive values. The principal stretch ratio in the uniaxial direction, 𝜆1, is then given by 𝐿0 + Δ𝐿 𝐿0 𝜆1 = with 𝐿0 being the initial length and 𝐿 being the actual length. applied force initial area = A0 change in gauge length gauge length = ∆L Figure M218-2 The stress versus strain curve can used instead of the force versus the change in the gauge length by setting the gauge length, thickness, and width to unity (1.0) and defining the engineering strain in place of the change in gauge length and the nominal (engineering) stress in place of the force. *MAT_077_O is a better alternative for fitting data resembling the curve above. *MAT_027 will provide a poor fit to a curve that exhibits a strong upturn in slope as strains become large. Alternatively, the stress versus strain curve can also be input by setting the gauge length, thickness, and width to unity (1.0) and defining the engineering strain in place of the change in gauge length and the nominal (engineering) stress in place of the force, see Figure M218-1. The least square fit to the experimental data is performed during the initialization phase and is a comparison between the fit and the actual input is provided in the d3hsp file. It is a good idea to visually check to make sure it is acceptable. The coefficients 𝐴 and 𝐵 are also printed in the output file. It is also advised to use the material driver for checking out the material model. *MAT_219 This is material type 219. This material model is the second generation of the UBC Composite Damage Model (CODAM2) for brick, shell, and thick shell elements developed at The University of British Columbia. The model is a sub-laminate-based continuum damage mechanics model for fiber reinforced composite laminates made up of transversely isotropic layers. The material model includes an optional non-local averaging and element erosion. Card 1 1 Variable MID 2 RO Type A8 F 3 EA F 4 EB F 5 6 7 8 PRBA PRCB F F Default none none none none none none Card 2 1 2 3 4 5 Variable GAB NLAYER R1 Type F Default none Card 3 Variable 1 XP Type F 2 YP F 3 ZP F I 0 4 A1 F 6 R2 F F 0.0 0.0 5 A2 F 6 A3 F 7 8 NFREQ I 0 7 AOPT I 0 8 Default 0.0 0.0 0.0 0.0 0.0 0.0 Variable 1 V1 Type F 2 V2 F 3 V3 F 4 D1 F 5 D2 F 6 D3 F *MAT_CODAM2 7 8 BETA MACF F I 0 Default 0.0 0.0 0.0 0.0 0.0 0.0 0.0 Angle Cards. For each of the NLAYER layers specify on angle. Include as many cards as needed to set NLAYER values. Card 5 1 2 3 4 5 6 7 8 Variable ANGLE1 ANGLE2 ANGLE3 ANGLE4 ANGLE5 ANGLE6 ANGLE7 ANGLE8 Type F F F F F F F F Default none none none none none none none none Card 6 1 2 3 4 5 6 7 8 Variable IMATT IFIBT ILOCT IDELT SMATT SFIBT SLOCT SDELT Type F F F F F F F F Default none none none none none none none none Card 7 1 2 3 4 5 6 7 8 Variable IMATC IFIBC ILOCC IDELC SMATC SFIBC SLOCC SDELC Type F F F F F F F F Default none none none none none none none none Card 8 1 2 3 4 5 6 7 8 Variable ERODE ERPAR1 ERPAR2 RESIDS Type Default I 0 F F none none F 0 VARIABLE DESCRIPTION MID RO EA EB PRBA PRCB GAB Material identification. A unique number or label not exceeding 8 characters must be specified. Mass density 𝐸𝑎, Young’s modulus in 𝑎-direction. This is the modulus along the direction of fibers. 𝐸𝑏, Young’s modulus in 𝑏-direction. This is the modulus transverse to fibers. 𝜈𝑏𝑎, Poisson’s ratio, 𝑏𝑎 (minor in-plane Poisson’s ratio). 𝜈𝑐𝑏, Poisson’s ratio, 𝑐𝑏 (Poisson’s ratio in the plane of isotropy). 𝐺𝑏𝑎, Shear modulus, 𝑎𝑏 (in-plane shear modulus). NLAYER Number of layers in the sub-laminate excluding symmetry. As an example, in a [0/45/-45/90]3s, NLAYER = 4. R1 R2 NFREQ Non-local averaging radius. Currently not used. Number of time steps between update of neighbor list for nonlocal smoothing. EQ.0: Do only one search at the start of the calculation XP, YP, ZP Coordinates of point 𝐩 for AOPT = 1 and 4. A1, A2, A3 Components of vector 𝐚 for AOPT = 2. AOPT *MAT_CODAM2 DESCRIPTION Material axes option : EQ.0.0: locally orthotropic with material axes determined by element nodes 1, 2, and 4, as with *DEFINE_COORDI- NATE_NODES, and then, for shells only, rotated about the shell element normal by an angle BETA. EQ.1.0: locally orthotropic with material axes determined by a point in space and the global location of the element center; this is the 𝑎-direction. This option is for solid elements only. EQ.2.0: globally orthotropic with material axes determined by vectors defined below, as with *DEFINE_COORDI- NATE_VECTOR. EQ.3.0: locally orthotropic material axes determined by rotating the material axes about the element normal by an angle, BETA, from a line in the plane of the element defined by the cross product of the vector 𝐯 with the element normal. EQ.4.0: locally orthotropic in cylindrical coordinate system with the material axes determined by a vector 𝐯, and an originating point, 𝐩, which define the centerline ax- is. This option is for solid elements only. LT.0.0: the absolute value of AOPT is a coordinate system ID number (CID on *DEFINE_COORDINATE_NODES, *DEFINE_COORDINATE_SYSTEM or *DEFINE_CO- ORDINATE_VECTOR). V1, V2, V3 Components of vector v for AOPT = 3 and 4. D1, D2, D3 Components of vector d for AOPT = 2. BETA Material angle in degrees for AOPT = 0 (shells only) and AOPT = 3. BETA be overridden on the element card, see *ELE- MENT_SHELL_BETA or *ELEMENT_SOLID_ORTHO. VARIABLE DESCRIPTION MACF Material axes change flag for brick elements: EQ.1: No change, default, EQ.2: switch material axes 𝑎 and 𝑏, EQ.3: switch material axes 𝑎 and 𝑐, EQ.4: switch material axes 𝑏 and 𝑐. ANGLEi Rotation angle in degrees of layers with respect to the material axes. Input one for each layer. IMATT IFIBT ILOCT IDELT SMATT SFIBT SLOCT SDELT IMATC IFIBC Initiation strain for damage in matrix (transverse) under tensile condition. Initiation strain for damage in the fiber (longitudinal) under tensile condition. Initiation strain for the anti-locking mechanism. This parameter should be equal to the saturation strain for the fiber damage mechanism under tensile condition. Not working in the current version. Can be used for visualization purpose only. Saturation strain for damage in matrix (transverse) under tensile condition. Saturation strain for damage in the fiber (longitudinal) under tensile condition. Saturation strain for the anti-locking mechanism under tensile condition. The recommended value for this parameter is (ILOCT+0.02). Not working in the current version. Can be used for visualization purpose only. Initiation strain for damage compressive condition. in matrix (transverse) under Initiation strain for damage in the fiber (longitudinal) under compressive condition. ILOCC IDELC SMATC SFIBC SLOCC SDELC ERODE *MAT_CODAM2 DESCRIPTION Initiation strain for the anti-locking mechanism. This parameter should be equal to the saturation strain for the fiber damage mechanism under compressive condition. Initiation strain for delamination. Not working in the current version. Can be used for visualization purpose only. Saturation strain for damage in matrix (transverse) under compressive condition. Saturation strain for damage in the fiber (longitudinal) under compressive condition. Saturation strain for compressive condition. parameter is (ILOCC + 0.02). the anti-locking mechanism under The recommended value for this Delamination strain. Not working in the current version. Can be used for visualization purpose only. Erosion Flag EQ.0: Erosion is turned off. EQ.1: Non-local strain based erosion criterion. EQ.2: Local strain based erosion criterion. EQ.3: Use both ERODE = 1 and ERODE = 2 criteria. ERPAR1 ERPAR2 The erosion parameter #1 used in ERODE types 1 and 3. ERPAR1>=1.0 and the recommended value is ERPAR1 = 1.2. The erosion parameter #2 used in ERODE types 2 and 3. The recommended value is five times SLOCC defined in cards 7 and 8. RESIDS Residual strength for layer damage Model Description: CODAM2 is developed for modeling the nonlinear, progressive damage behavior of laminated fiber-reinforced plastic materials. The model is based on the work by (Forghani, 2011; Forghani et al. 2011a; Forghani et al. 2011b) and is an extension of the original model, CODAM (Williams et al. 2003). Briefly, the model uses a continuum damage mechanics approach and the following assumptions have been made in its development: 1. The material is an orthotropic medium consisting of a number of repeating units through the thickness of the laminate, called sub-laminates. e.g. [0/±45/90] in a [0/±45/90]8S laminate. 2. The nonlinear behavior of the composite sub-laminate is only caused by damage evolution. Nonlinear elastic or plastic deformations are not consid- ered. Formulation: The in-plane secant stiffness of the damaged laminate is represented as the summation of the effective contributions of the layers in the laminate as shown. 𝐀𝑑 = ∑ 𝑡𝑘𝚻𝑘 T𝐐𝑘 𝑑𝚻𝑘 𝑑 is the in-plane secant where 𝚻𝑘 is the transformation matrix for the strain vector, and 𝐐𝑘 stiffness of kth layer in the principal orthotropic plane, and 𝑡𝑘 is the thickness of the kth layer of an 𝑛-layered laminate. A physically-based and yet simple approach has been employed here to derive the damaged stiffness matrix. Two reduction coefficients, 𝑅𝑓 and 𝑅𝑚, that represent the reduction of stiffness in the longitudinal (fiber) and transverse (matrix) directions have been employed. The shear modulus has also been reduced by the matrix reduction parameter. The major and minor Poisson’s ratios have been reduced by 𝑅𝑓 and 𝑅𝑚re- spectively. A sub-laminate-level reduction, 𝑅𝐿, is incorporated to avoid spurious stress locking in the damaged zone. This would lead to an effective reduced stiffness matrix 𝑑. The reduction coefficients are equal to 1 in the undamaged condition and gradually 𝐐𝑘 decrease to 0 for a saturated damage condition. 𝐐𝑘 𝑑 = 𝑅𝐿 𝜈12𝜈21 𝐸1 (𝑅𝑓 ) (𝑅𝑚) 𝜈12𝐸2 ⎡ ⎢ 1 − (𝑅𝑓 ) ⎢ ⎢ (𝑅𝑚) (𝑅𝑓 ) ⎢ ⎢ ⎢ (𝑅𝑚) 1 − (𝑅𝑓 ) ⎢ ⎢ ⎢ ⎣ 𝜈12𝜈21 𝜈12𝐸2 (𝑅𝑚) (𝑅𝑚) 𝐸2 (𝑅𝑓 ) 1 − (𝑅𝑓 ) (𝑅𝑚) (𝑅𝑚) 1 − (𝑅𝑓 ) 𝜈12𝜈21 𝜈12𝜈21 (𝑅𝑚) 𝑑T = 𝐐𝑘 ⎤ ⎥ ⎥ ⎥ ⎥ ⎥ ⎥ ⎥ ⎥ ⎥ 𝐺12⎦ where 𝐸1, 𝐸2, 𝜈12, 𝜈21, and 𝐺12 are the elastic constants of the lamina. *MAT_CODAM2 In CODAM2, the evolution of damage mechanisms are expressed in terms of equivalent strain parameters. The equivalent strain function that governs the fiber stiffness reduction parameter is written in terms of the longitudinal normal strains by eq = 𝜀11,𝑘, 𝜀𝑓 ,𝑘 𝑘 = 1, . . . , 𝑛 The equivalent strain function that governs the matrix stiffness reduction parameter is written in an interactive form in terms of the transverse and shear components of the local strain. eq = sign(𝜀22,𝑘)√(𝜀22,𝑘)2 + ( 𝜀𝑚,𝑘 𝛾12,𝑘 ) , 𝑘 = 1, . . . , 𝑛 The sign of the transverse normal strain plays a very important role in the initiation and growth of damage since it indicates the compressive or tensile nature of the transverse stress. Therefore, the equivalent strain for the matrix damage carries the sign of the transverse normal strain. Evolution of the overall damage mechanism (anti-locking) is written in terms of the maximum principal strains. eq = max[prn(ε)] 𝜀𝐿 Within the framework of non-local strain-softening formulations adopted here, all damage modes, be it intra-laminar (i.e. fiber and matrix damage) or overall sub- laminate modes are considered to be a function of the non-local (averaged) equivalent strain defined as: eq = ∫ 𝜀𝛼 𝜀̅𝛼 Ω𝐗 eq(𝐱)𝑤𝛼(𝐗 − 𝐱)𝑑Ω where the subscript 𝛼 denotes the mode of damage: fiber (𝛼 = 𝑓 ) and matrix (𝛼 = 𝑚) damage in each layer, 𝑘, within the sub-laminate or associated with the overall sub- eq and laminate, namely, locking (𝛼 = 𝐿). Thus, for a given sub-laminate with n layers,𝜀𝛼 eq are vectors of size 2𝑛 + 1. 𝐗 represents the position vector of the original point of 𝜀̅𝛼 interest and 𝐱 denotes the position vector of all other points (Gauss points) in the averaging zone denoted by Ω. In classical isotropic non-local averaging approach, this zone is taken to be spherical (or circular in 2D) with a radius of r (named R1 in the material input card). The parameter, 𝑟, which affects the size of the averaging zone, introduces a length scale into the model that is linked directly to the predicted size of the damage zone. Averaging is done with a bell-shaped weight function, 𝑤𝛼, evaluated by 𝑤𝛼 = ⎢⎡1 − ( ⎣ ) ⎥⎤ ⎦ ε i ε s eq (a) (b) Figure M219-1. illustrations of (a) damage parameter and (b) reduction parameter. where 𝑑 is the distance from the integration point of interest to another integration point with the averaging zone. The damage parameters, 𝜔, are calculated as a function of the corresponding averaged equivalent strains. In CODAM2 the damage parameters are assumed to grow as a hyperbolic function of the damage potential (non-local equivalent strains) such that when used in conjunction with stiffness reduction factors that vary linearly with the damage parameters they result in a linear strain-softening response (or a bilinear stress- strain curve) for each mode of damage eq∣ − 𝜀𝛼 𝑖 ) 𝑖 ) 𝑠 − 𝜀𝛼 eq∣ − 𝜀𝛼 ∣𝜀̅𝛼 (∣𝜀̅𝛼 (𝜀𝛼 𝑖 > 0 𝜔𝛼 = , 𝜀𝛼 𝑒𝑞∣ ∣𝜀̅𝛼 where superscripts 𝑖 and 𝑠 denote, respectively, the damage initiation and saturation values of the strain quantities to which they are assigned. The initiation and saturation parameters are defined in material cards #6 and #7. Damage is considered to be a monotonically increasing function of time, t, such that 𝜔𝛼 = max τ<t (𝜔𝛼 𝜏) where 𝜔𝛼 of damage at previous times 𝜏 ≤ 𝑡. 𝑡 is the value of 𝜔𝛼 for the current time (load state), and 𝜔𝛼 𝜏 represents the state Damage is applied by scaling the layer stress by reduction parameters 𝑅𝛼 = 1 − 𝜔𝛼 where 𝛼 = 𝑓 and 𝛼 = 𝑚. The layer stresses are summed and then then scaled by reduction parameter 𝑅𝐿 = 1 − 𝜔𝐿. Figures M219-1 (a) and (b) show the relationship between the damage and reduction parameters If the parameter RESIDS > 0, damage in the layers is limited such that 𝑅𝑓 = max(RESIDS, 1 − 𝜔𝑓 ) 𝑅𝑚 = max(RESIDS, 1 − 𝜔𝑚) Element Erosion: When ERODE > 0, an erosion criterion is checked at each integration point. Shell elements and thick shell elements will be deleted when the erosion criterion has been met at all integration points. Brick elements will be deleted when the erosion criterion is met at any of the integration points. For ERODE = 1, the erosion criterion is met when maximum principal strain exceeds either SLOCT × ERPAR1 for elements in tension, or SLOCC × ERPAR1 for elements in compression. Elements are in tension when the magnitude of the first principal strain is greater than the magnitude of the third principal strain and in compression when the third principal strain is larger. When 𝑅 > 0, the ERODE = 1 criterion is checked using the non-local (averaged) principal strain. For ERODE = 2, the erosion criterion is met when the local (non- averaged) maximum principal strain exceeds ERPAR2. For ERODE = 3, both of these erosion criteria are checked. For visualization purposes, the ratio of the maximum principal strain over the limit is stored in the location of plastic strain which is written by default to the elout and d3plot files. History Variables: History variables for CODAM2 are enumerated in the following tables. To include them in the D3PLOT database, use NEIPH (bricks) or NEIPS (shells) on *DATABASE_- EXTENT_BINARY. For brick elements, add 4 to the variable numbers in the table because the first 6 history variables are reserved. *MAT_219 VARIABLE # DESCRIPTION 3 4 5 6 7 8 ⋮ Overall (anti-locking) Damage. Delamination Damage (for visualization only) Fiber damage in the first layer Matrix damage in the first layer Fiber damage in the second layer Matrix damage in the second layer ⋮ 3 + 2 × NLAYER Fiber damage in the last layer 4 + 2 × NLAYER Matrix damage in the last layer Equivalent Strains used to evaluate damage (averaged if R1 > 0) DESCRIPTION VARIABLE # 5 + 2 × NLAYER 6 + 2 × NLAYER 7 + 2 × NLAYER 8 + 2 × NLAYER 9 + 2 × NLAYER ⋮ 4 + 4 × NLAYER 5 + 4 × NLAYER eq 𝜀𝑅 eq 𝜀𝑓 ,1 eq 𝜀𝑚,1 eq 𝜀𝑓 ,2 eq 𝜀𝑚,2 ⋮ eq 𝜀𝑓 ,𝑛 eq 𝜀𝑓 ,𝑛 *MAT_219 Total Strain VARIABLE # 6 + 4 × NLAYER 7 + 4 × NLAYER 8 + 4 × NLAYER 9 + 4 × NLAYER 10 + 4 × NLAYER 11 + 4 × NLAYER 𝜀𝑥 𝜀𝑦 𝜀𝑧 𝛾𝑥𝑦 𝛾𝑦𝑧 𝛾𝑧𝑥 *MAT_220 This is Material Type 220, a rigid material for shells or solids. Unlike *MAT_020, a *MAT_220 part can be discretized into multiple disjoint pieces and have each piece behave as an independent rigid body. The inertia properties for the disjoint pieces are determined directly from the finite element discretization. Nodes of a *MAT_220 part cannot be shared by any other rigid part. A *MAT_220 part may share nodes with deformable structural and solid elements. This material option can be used to model granular material where the grains interact through an automatic single surface contact definition. Another possible use includes modeling bolts as rigid bodies where the bolts belong to the same part ID. This model eliminates the need to represent each rigid piece with a unique part ID. 5 6 7 8 Card 1 Variable MID 2 RO Type A8 F 3 E F 4 PR F Default none none none none VARIABLE DESCRIPTION MID RO E PR Material identification. A unique number or label not exceeding 8 characters must be specified. Mass density. Young’s modulus. Poisson’s ratio. *MAT_ORTHOTROPIC_SIMPLIFIED_DAMAGE This is Material Type 221. An orthotropic material with optional simplified damage and optional failure for composites can be defined. This model is valid only for 3D solid elements, with reduced or full integration. The elastic behavior is the same as MAT_022. Nine damage variables are defined such that damage is different in tension and compression. These damage variables are applicable to 𝐸𝑎, 𝐸𝑏, 𝐸𝑐, 𝐺𝑎𝑏, 𝐺𝑏𝑐 and 𝐺𝑐𝑎. In addition, nine failure criteria on strains are available. When failure occurs, elements are deleted (erosion). Failure depends on the number of integration points failed through the element. See the material description below. Card 1 1 Variable MID 2 RO Type A8 F 3 EA F 4 EB F 5 EC F 6 7 8 PRBA PRCA PRCB F F F Default none none none none none none none none Card 2 1 2 3 4 5 6 7 8 Variable GAB GBC GCA AOPT MACF Type F F F Default none none none Card 3 Variable 1 XP Type F 2 YP F 3 ZP F 4 A1 F F 0.0 5 A2 F I 0 6 A3 F Default 0.0 0.0 0.0 0.0 0.0 0.0 7 Card 4 Variable 1 V1 Type F 2 V2 F 3 V3 F 4 D1 F 5 D2 F 6 D3 F 7 8 BETA F Default 0.0 0.0 0.0 0.0 0.0 0.0 0.0 Card 5 1 2 3 4 5 6 7 8 Variable NERODE NDAM EPS1TF EPS2TF EPS3TF EPS1CF EPS2CF EPS3CF Type Default I 0 Card 6 1 I 0 2 F F F F F F 1020 1020 1020 -1020 -1020 -1020 3 4 5 6 7 8 Variable EPS12F EPS23F EPS13F EPSD1T EPSC1T CDAM1T EPSD2T EPSC2T Type F F F Default 1020 1020 1020 F 0. F 0. F 0. F 0. F 0. Card 7 1 2 3 4 5 6 7 8 Variable CDAM2T EPSD3T EPSC3T CDAM3T EPSD1C EPSC1C CDAM1C EPSD2C Type I Default 0. I 0. F 0. F 0. F 0. F 0. F 0. F 0. Card 8 1 2 3 4 5 6 7 8 Variable EPSC2C CDAM2C EPSD3C EPSC3C CDAM3C EPSD12 EPSC12 CDAM12 Type F Default 0. F 0. F 0. F 0. F 0. F 0. F 0. F 0. Card 9 1 2 3 4 5 6 7 8 Variable EPSD23 EPSC23 CDAM23 EPSD31 EPSC31 CDAM31 Type F Default 0. F 0. F 0. F 0. F 0. F 0. VARIABLE DESCRIPTION MID RO EA EB EC PRBA PRCA PRCB GAB GBC GCA Material identification. A unique number or label not exceeding 8 characters must be specified. Mass density 𝐸𝑎, Young’s modulus in 𝑎-direction 𝐸𝑏, Young’s modulus in 𝑏-direction 𝐸𝑐, Young’s modulus in 𝑐-direction 𝜈𝑏𝑎, Poisson ratio 𝜈𝑐𝑎, Poisson ratio 𝜈𝑐𝑏, Poisson ratio 𝐺𝑎𝑏, Shear modulus 𝐺𝑏𝑐, Shear modulu 𝐺𝑐𝑎, Shear modulus VARIABLE AOPT DESCRIPTION Material axes option : EQ.0.0: locally orthotropic with material axes determined by element nodes 1, 2, and 4, as with *DEFINE_ COORDINATE_NODES. EQ.1.0: locally orthotropic with material axes determined by a point in space and the global location of the element center; this is the 𝑎-direction. This option is for solid elements only. EQ.2.0: globally orthotropic with material axes determined by *DEFINE_ as with below, vectors COORDINATE_VECTOR. defined EQ.3.0: locally orthotropic material axes determined by rotating the material axes about the element normal by an angle, BETA, from a line in the plane of the element defined by the cross product of the vector 𝐯 with the element normal. EQ.4.0: locally orthotropic in cylindrical coordinate system with the material axes determined by a vector 𝐯, and an originating point, 𝐩, which define the centerline ax- is. This option is for solid elements only. LT.0.0: the absolute value of AOPT is a coordinate system ID number (CID on *DEFINE_COORDINATE_NODES, *DEFINE_ *DEFINE_COORDINATE_SYSTEM COORDINATE_VECTOR). or MACF Material axes change flag for brick elements: EQ.1: No change, default, EQ.2: switch material axes 𝐚 and 𝐛, EQ.3: switch material axes 𝐚 and 𝐜, EQ.4: switch material axes 𝐛 and 𝐜. XP, YP, ZP Coordinates of point 𝐩 for AOPT = 1 and 4 A1, A2, A3 Components of vector 𝐚 for AOPT = 2 V1, V2, V3 Components of vector 𝐯 for AOPT = 3 and 4 D1, D2, D3 Components of vector 𝐝 for AOPT = 2 BETA NERODE *MAT_ORTHOTROPIC_SIMPLIFIED_DAMAGE DESCRIPTION Material angle in degrees for AOPT = 3, may be overridden on the element card, see *ELEMENT_SOLID_ORTHO. Element erosion flag. For multi-integration point elements, each of the failure strains mentioned below for NERODE 2 and higher need only occur in one integration point to trigger element erosion, and for NERODE values 6 to 11, which require more than one failure strain be reached, those failure strains need not occur in the same integration point. EQ.0: No erosion (default). EQ.1: Erosion occurs when one failure strain is reached in all integration points. EQ.2: Erosion occurs when one failure strain is reached. EQ.3: Erosion occurs when a tension or compression failure strain in the 𝑎-direction is reached. EQ.4: Erosion occurs when as a tension or compression failure strain in the 𝑏-direction is reached. EQ.5: Erosion occurs when a tension or compression failure strain in the 𝑐-direction is reached. EQ.6: Erosion occurs when tension or compression failure strain in both the 𝑎- and 𝑏-directions are reached. EQ.7: Erosion occurs when tension or compression failure strain in both the 𝑏- and 𝑐-directions are reached. EQ.8: Erosion occurs when tension or compression failure strain in both the 𝑎- and 𝑐-directions are reached. EQ.9: Erosion occurs when tension or compression failure strain in all 3 directions are reached. EQ.10:Erosion occurs when tension or compression failure strain in both the 𝑎- and 𝑏-directions are reached and either of the out-of-plane failure shear strains (bc or ac) is reached. . EQ.11:Erosion occurs when tension failure strain in either the 𝑎- or 𝑏-directions is reached and either of the out-of-plane failure shear strains (bc or ac) is reached. VARIABLE DESCRIPTION NDAM Damage flag: EQ.0: No damage (default) EQ.1: Damage in tension only (null for compression) EQ.2: Damage in tension and compression EPS1TF Failure strain in tension along the 𝑎-direction EPS2TF Failure strain in tension along the 𝑏-direction EPS3TF Failure strain in tension along the 𝑐-direction EPS1CF Failure strain in compression along the 𝑎-direction EPS2CF Failure strain in compression along the 𝑏-direction EPS3CF Failure strain in compression along the 𝑐-direction EPS12F Failure shear strain in the 𝑎𝑏-plane EPS23F Failure shear strain in the 𝑏𝑐-plane EPS13F Failure shear strain in the 𝑎𝑐-plane EPSD1T EPSC1T 𝑠 Damage threshold in tension along the 𝑎-direction, 𝜀1𝑡 𝑐 Critical damage threshold in tension along the 𝑎-direction, 𝜀1𝑡 CDAM1T 𝑐 Critical damage in tension along the 𝑎-direction, 𝐷1𝑡 EPSD2T EPSC2T 𝑠 Damage threshold in tension along the 𝑏-direction, 𝜀2𝑡 𝑐 Critical damage threshold in tension along the b-direction, 𝜀2𝑡 CDAM2T 𝑐 Critical damage in tension along the 𝑏-direction, 𝐷2𝑡 EPSD3T EPSC3T 𝑠 Damage threshold in tension along the 𝑐-direction, 𝜀3𝑡 𝑐 Critical damage threshold in tension along the 𝑐-direction, 𝜀3𝑡 CDAM3T 𝑐 Critical damage in tension along the 𝑐-direction, 𝐷3𝑡 EPSD1C EPSC1C 𝑠 Damage threshold in compression along the 𝑎-direction, 𝜀1𝑐 Critical damage threshold in compression along the 𝑎-direction, 𝑐 𝜀1𝑐 *MAT_ORTHOTROPIC_SIMPLIFIED_DAMAGE DESCRIPTION CDAM1C 𝑐 Critical damage in compression along the 𝑎-direction, 𝐷1𝑐 EPSD2C EPSC2C 𝑠 Damage threshold in compression along the 𝑏-direction, 𝜀2𝑐 Critical damage 𝑐 direction, 𝜀2𝑐 threshold in compression along the 𝑏- CDAM2C 𝑐 Critical damage in compression along the 𝑏-direction, 𝐷2𝑐 EPSD3C EPSC3C 𝑠 Damage threshold in compression along the 𝑐-direction, 𝜀3𝑐 Critical damage threshold in compression along the 𝑐-direction, 𝑐 𝜀3𝑐 CDAM3C 𝑐 Critical damage in compression along the 𝑐-direction, 𝐷3𝑐 EPSD12 EPSC12 𝑠 Damage threshold for shear in the 𝑎𝑏-plane, 𝜀12 𝑐 Critical damage threshold for shear in the 𝑎𝑏-plane, 𝜀12 CDAM12 𝑐 Critical damage for shear in the 𝑎𝑏-plane, 𝐷12 EPSD23 EPSC23 𝑠 Damage threshold for shear in the 𝑏𝑐-plane, 𝜀23 𝑐 Critical damage threshold for shear in the 𝑏𝑐-plane, 𝜀23 CDAM23 𝑐 Critical damage for shear in the 𝑏𝑐-plane, 𝐷23 EPSD31 EPSC31 𝑠 Damage threshold for shear in the 𝑎𝑐-plane, 𝜀31 𝑐 Critical damage threshold for shear in the 𝑎𝑐-plane, 𝜀31 CDAM31 𝑐 Critical damage for shear in the 𝑎𝑐-plane, 𝐷31 Remarks: If 𝜀𝑘 𝑐 < 𝜀𝑘 𝑠 , no damage is considered. Failure occurs only when failure strain is reached. Failure can occur along the 3 orthotropic directions, in tension, in compression and for shear behavior. Nine failure strains drive the failure. When failure occurs, elements are deleted (erosion). Under the control of the NERODE flag, failure may occur either when only one integration point has failed, when several integration points have failed or when all integrations points have failed. Damage applies to the 3 Young’s moduli and the 3 shear moduli. Damage is different for tension and compression. Nine damage variables are used: 𝑑1𝑡, 𝑑2𝑡, 𝑑3𝑡, 𝑑1𝑐, 𝑑2𝑐, 𝑑3𝑐, 𝑑12, 𝑑23, 𝑑13. The damaged flexibility matrix is: 𝐸𝑎(1 − 𝑑1[𝑡,𝑐]) −𝜐𝑏𝑎 𝐸𝑏 −𝜐𝑐𝑎 𝐸𝑐 −𝜐𝑏𝑎 𝐸𝑏 𝐸𝑏(1 − 𝑑2[𝑡,𝑐]) −𝜐𝑐𝑏 𝐸𝑐 −𝜐𝑐𝑎 𝐸𝑐 −𝜐𝑐𝑏 𝐸𝑐 𝐸𝑐(1 − 𝑑3[𝑡,𝑐]) 𝐺𝑎𝑏(1 − 𝑑12) 𝐺𝑏𝑐(1 − 𝑑23) 𝑆dam = ⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎛ ⎝ The nine damage variables are calculated as follows: 𝑑𝑘 = max (𝑑𝑘; 𝐷𝑘 𝑐 ⟨ 𝜀𝑘 − 𝜀𝑘 𝑠 ⟩ 𝑐 − 𝜀𝑘 𝜀𝑘 + ) ⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎞ 𝐺𝑐𝑎(1 − 𝑑31)⎠ with k = 1t, 2t, 3t, 1c, 2c, 3c, 12, 23, 31. ⟨ ⟩+ is the positive part: ⟨𝑥⟩+ = { if x > 0 if x < 0 . Damage in compression may be deactivated with the NDAM flag. In this case, damage in compression is null, and only damage in tension and for shear behavior are taken into account. The nine damage variables may be post-processed through additional variables. The number of additional variables for solids written to the d3plot and d3thdt databases is input by the optional *DATABASE_EXTENT_BINARY card as variable NEIPH. These additional variables are tabulated below: History Variable Description Value 𝑑1𝑡 𝑑2𝑡 𝑑3𝑡 𝑑1𝑐 𝑑2𝑐 𝑑3𝑐 𝑑12 damage in traction along 𝑎 damage in traction along 𝑏 damage in traction along 𝑐 damage in compression along 𝑎 0 - no damage damage in compression along 𝑏 damage in compression along 𝑐 0 < 𝑑𝑘 < 𝐷𝑘 𝑐 - damage shear damage in 𝑎𝑏-plane LS-PrePost History Variable plastic strain 1 2 3 4 5 History Variable Description Value 𝑑23 𝑑13 shear damage in 𝑏𝑐-plane shear damage in 𝑎𝑐-plane LS-PrePost History Variable 7 8 The first damage variable is stored as in the place of effective plastic strain. The eight other damage variables may be plotted in LS-PrePost as element history variables. *MAT_TABULATED_JOHNSON_COOK This is Material Type 224. An elasto-viscoplastic material with arbitrary stress versus strain curve(s) and arbitrary strain rate dependency can be defined. Plastic heating causes adiabatic temperature increase and material softening. Optional plastic failure strain can be defined as a function of triaxiality, strain rate, temperature and/or element size. Please take careful note the sign convention of triaxiality used for *MAT_224 as illustrated in Figure M224-1. This material model resembles the original Johnson-Cook material but with the possibility of general tabulated input parameters. An equation of state (*EOS) is optional for solid elements, tshell formulations 3 and 5, and 2D continuum elements, and is invoked by setting EOSID to a nonzero value in *PART. If an equation of state is used, only the deviatoric stresses are calculated by the material model and the pressure is calculated by the equation of state. Card 1 1 Variable MID 2 RO Type A8 F 3 E F 4 PR F 5 CP F 6 TR F 7 8 BETA NUMINT F F Default none none none none none 0.0 1.0 1.0 Card 2 1 2 3 4 5 Variable LCK1 LCKT LCF LCG LCH Type Default F 0 F 0 F 0 F 0 F 0 6 LCI F 0 7 *MAT_TABULATED_JOHNSON_COOK Card 3 1 2 3 4 5 6 7 8 Variable FAILOPT NUMAVG NCYFAIL ERODE LCPS Type F F F F F VARIABLE DESCRIPTION MID RO E PR CP TR Material identification. A unique number or label not exceeding 8 characters must be specified. Mass density. Young’s modulus: GT.0.0: constant value is used LT.0.0: -E gives curve ID for temperature dependence Poisson’s ratio. Specific heat (superseded by heat capacity in *MAT_THERMAL_ OPTION if a coupled thermal/structural analysis). Room temperature. BETA Fraction of plastic work converted into heat: GT.0.0: constant value is used LT.0.0: -BETA gives either a curve ID for strain rate dependence or a table ID for strain rate and tempera- ture dependence. VARIABLE NUMINT DESCRIPTION GT.0.0: Number of integration points which must fail before the element is deleted. Available for shells and sol- ids. LT.0.0: -NUMINT is percentage of integration points/layers which must fail before shell element fails. For fully integrated shells, a methodology is used where a lay- er fails if one integration point fails and then the giv- en percentage of layers must fail before the element fails. Only available for shells except as noted below EQ.-200: Turns off erosion for shells and solids. recommended unless used *CONSTRAINED_TIED_NODES_FAILURE. Not in conjunction with LCK1 LCKT LCF LCG LCH Load curve ID or Table ID. The load curve ID defines effective stress as a function of effective plastic strain. The table ID defines for each plastic strain rate value a load curve ID giving the (isothermal) effective stress versus effective plastic strain for that rate. As in *MAT_024, natural logarithmic strain rates can be used by setting the first strain rate to a negative value. Table ID defining for each temperature value a load curve ID giving the (quasi-static) effective stress versus effective plastic strain for that temperature. Load curve ID or Table ID. The load curve ID defines plastic failure strain (or scale factor – see Remarks) as a function of triaxiality. The table ID defines for each Lode parameter a load curve ID giving the plastic failure strain versus triaxiality for that Lode parameter. (Table option only for solids and not yet generally supported). See Remarks for a description of the combination of LCF, LCG, LCH, and LCI. Load curve ID defining plastic failure strain (or scale factor – see Remarks) as a function of plastic strain rate. If the first abscissa value in the curve corresponds to a negative strain rate, LS- DYNA assumes that the natural logarithm of the strain rate value is used for all abscissa values. See Remarks for a description of the combination of LCF, LCG, LCH, and LCI. Load curve ID defining plastic failure strain (or scale factor – see Remarks) as a function of temperature. See Remarks for a description of the combination of LCF, LCG, LCH, and LCI. LCI *MAT_TABULATED_JOHNSON_COOK DESCRIPTION Load curve ID, Table ID, or Table_3D ID. The load curve ID defines plastic failure strain (or scale factor – see Remarks) as a function of element size. The table ID defines for each triaxiality a load curve ID giving the plastic failure strain versus element size for that triaxiality. If a three dimensional table ID is referred, plastic failure strain can be a function of Lode parameter (TABLE_3D), triaxiality (TABLE), and element size (CURVE). See Remarks for a description of the combination of LCF, LCG, LCH, and LCI. FAILOPT Flag for additional failure criterion 𝐹2, see Remarks. EQ.0.0: off (default) EQ.1.0: on NUMAVG NCYFAIL Number of time steps for running average of plastic failure strain in the additional failure criterion. Default is 1 (no averaging). Number of time steps that the additional failure criterion must be met before element deletion. Default is 1. ERODE Erosion flag (only for solid elements): EQ.0.0: default, element erosion is allowed. EQ.1.0: element does not erode; deviatoric stresses set to zero when element fails. Table ID with first principal stress limit as function of plastic strain (curves) and plastic strain rate (table). This option is for post-processing purposes only and gives an indication of areas in the structure where failure is likely to occur. History variable #17 shows a value of 1.0 for integration points that exceeded the limit, else a value of 0.0. LCPS Remarks: The flow stress 𝜎𝑦 is expressed as a function of plastic strain 𝜀𝑝, plastic strain rate 𝜀̇𝑝 and temperature 𝑇 via the following formula (using load curves/tables LCK1 and LCKT): 𝑠𝑦 = 𝑘1(𝜀𝑝, 𝜀̇𝑝) 𝑘𝑡(𝜀𝑝, 𝑇) 𝑘𝑡(𝜀𝑝, 𝑇𝑅) Note that 𝑇𝑅 is a material parameter and should correspond to the temperature used when performing the room temperature tensile tests. If simulations are to be performed plastic failure strain tension compression -2/3 -1/3 triaxiality p/σ vm 1/3 2/3 Figure M224-1. Typical failure curve for metal sheet, modeled with shell elements. with an initial temperature TI deviating from 𝑇𝑅 then this temperature should be set using *INITIAL_STRESS_SOLID/SHELL by setting history variable #14 for solid elements or history variable #10 for shell elements. Optional plastic failure strain is defined as a function of triaxiality parameter, plastic strain rate element area for shells and volume over maximum area for solids) by 𝑝/𝜎𝑣𝑚, Lode 𝜀̇𝑝, temperature 𝑇 and initial element size 𝑙c (square root of 𝜀𝑝𝑓 = 𝑓 ( 𝜎vm , 27𝐽3 2𝜎vm 3 ) 𝑔(𝜀̇𝑝)ℎ(𝑇)𝑖 (𝑙𝑐, 𝜎vm ) using load curves/tables LCF, LCG, LCH and LCI. If more than one of these four variables LCF, LCG, LCH and LCI are defined, be aware that the net plastic failure strain is essentially the product of multiple functions as shown in the above equation. This means that one and only one of the variables LCF, LCG, LCH, and LCI can point to curve(s) that have plastic strain along the curve ordinate. The remaining nonzero variable(s) LCF, LCG, LCH, and LCI should point to curve(s) that have a unitless scaling factor along the curve ordinate. A typical failure curve LCF for metal sheet, modeled with shell elements is shown in Figure M224-1. Triaxiality should be monotonically increasing in this curve. A reasonable range for triaxiality is -2/3 to 2/3 if shell elements are used (plane stress). For 3-dimensional stress states (solid elements), the possible range of triaxiality goes from -∞ to +∞, but to get a good resolution in the internal load curve discretization (depending on parameter LCINT of *CONTROL_SOLUTION) one should define lower limits, e.g. -1 to 1 if LCINT = 100 (default). The default failure criterion of this material model depends on plastic strain evolution 𝜀̇𝑝 and on plastic failure strain 𝜀𝑝𝑓 and is obtained by accumulation over time: 𝐹 = ∫ 𝜀̇𝑝 𝜀𝑝𝑓 𝑑𝑡 where element erosion takes place when 𝐹 ≥ 1. This accumulation provides load-path dependent treatment of failure. The value of 𝐹 is stored as history variable #8 for shells and #12 for solids. An additional, load-path independent, failure criterion can be invoked by setting FAILOPT = 1, where the current state of plastic strain is used: 𝐹2 = 𝜀𝑝 𝜀𝑝𝑓 Two additional parameters can be used as countermeasures against stress oscillations for this failure criterion. With NUMAVG active, plastic failure strain is averaged over NUMAVG time steps for the 𝐹2 criterion. The value of 𝐹2, taking into account any averaging per NUMAVG, is stored as history variable #14 for shells and #16 for solids. NUMAVG cannot exceed 30. NCYFAIL defines the number of time steps that 𝐹2 ≥ 1 must be met before element deletion takes place. The number of time steps that 𝐹2 ≥ 1 is stored as history variable #15 for shells and #19 for solids. Temperature increase is caused by plastic work 𝑇 = 𝑇𝑅 + 𝐶𝑝𝜌 ∫ 𝜎𝑦𝜀̇𝑝𝑑𝑡 with room temperature 𝑇𝑅, dissipation factor 𝛽, specific heat 𝐶𝑝, and density 𝜌. For *CONSTRAINED_TIED_NODES_WITH_FAILURE, the failure is based on the damage instead to the plastic strain. History variables may be post-processed through additional variables. The number of additional variables for shells/solids written to the d3plot and d3thdt databases is input by the optional *DATABASE_EXTENT_BINARY card as variable NEIPS/NEIPH. The relevant additional variables of this material model are tabulated below: LS-PrePost history variable # 1 7 8 9 10 11 12 17 Shell elements plastic strain rate plastic work ratio of plastic strain to plastic failure strain element size temperature plastic failure strain triaxiality LCPS: critical value LS-PrePost history variable # 5 8 9 10 11 12 13 14 17 Solid elements plastic strain rate plastic failure strain triaxiality Lode parameter plastic work ratio of plastic strain to plastic failure strain element size temperature LCPS: critical value *MAT_TABULATED_JOHNSON_COOK_GYS This is Material Type 224_GYS. This is an isotropic elastic plastic material law with J3 dependent yield surface. This material considers tensile/compressive asymmetry in the material response, which is important for HCP metals like Titanium. The model is available for solid elements. Card 1 1 Variable MID 2 RO Type A8 F 3 E F 4 PR F 5 CP F 6 TR F 7 8 BETA NUMINT F F Default none none none none none 0.0 1.0 1.0 Card 2 1 2 3 4 5 Variable LCK1 LCKT LCF LCG LCH Type Default F 0 Card 3 1 F 0 2 F 0 3 F 0 4 F 0 5 6 LCI F 0 6 7 8 7 8 Variable LCCR LCCT LCSR LCST IFLAG SFIEPM NITER Type Default F 0 F 0 F 0 F 0 F 0 F 1 100 VARIABLE MID DESCRIPTION Material identification. A unique number or label not exceeding 8 characters must be specified. RO Mass density. VARIABLE DESCRIPTION E Young’s modulus: GT.0.0: constant value is used LT.0.0: temperature dependent Young’s modulus given by load curve ID = -E PR CP TR Poisson’s ratio. Specific heat. Room temperature. BETA Fraction of plastic work converted into heat. NUMINT Number of integration points which must fail before the element is deleted. LCK1 LCKT LCF LCG LCH LCI EQ.-200: Turns off erosion for solids. Not recommended unless used in conjunction with *CONSTRAINED_- TIED_NODES_FAILURE. Table ID defining for each plastic strain rate value a load curve ID giving the (isothermal) effective stress versus effective plastic strain for that rate. Table ID defining for each temperature value a load curve ID giving the (quasi-static) effective stress versus effective plastic strain for that temperature. Load curve ID or Table ID. The load curve ID defines plastic failure strain as a function of triaxiality. The table ID defines for each Lode parameter a load curve ID giving the plastic failure strain versus triaxiality for that Lode parameter. (Table option only for solids and not yet generally supported). Load curve ID defining plastic failure strain as a function of plastic strain rate. Load curve ID defining plastic failure strain as a function of temperature Load curve ID or Table ID. The load curve ID defines plastic failure strain as a function of element size. The table ID defines for each triaxiality a load curve ID giving the plastic failure strain versus element size for that triaxiality. VARIABLE LCCR LCCT LCSR LCST DESCRIPTION Table ID. The curves in this table define compressive yield stress as a function of plastic strain or effective plastic strain . The table ID defines for each plastic strain rate value or effective plastic strain rate value a load curve ID giving the (isothermal) compressive yield stress versus plastic strain or effective plastic strain for that rate. Table ID defining for each temperature value a load curve ID giving the (quasi-static) compressive yield stress versus strain for that temperature. The curves in this table define compressive yield stress as a function of plastic strain or effective plastic strain . Table ID. The load curves define shear yield stress in function of plastic strain or effective plastic strain .The table ID defines for each plastic strain rate value or effective plastic strain rate value a load curve ID giving the (isothermal) shear yield stress versus plastic strain or effective plastic strain for that rate. Table ID defining for each temperature value a load curve ID giving the (quasi-static) shear yield stress versus strain for that temperature. The load curves define shear yield stress as a function of plastic strain or effective plastic strain . IFLAG Flag to specify abscissa for LCCR, LCCT, LCSR, LCST: EQ.0.0: Compressive and shear yields are given in a function of plastic strain as defined in the remarks (default). EQ.1.0: Compressive and shear yields are given in function of effective plastic strain. SFIEPM Scale factor on the initial estimate of the plastic multiplier. NITER Number of secant iterations to be performed. Remarks: If IFLAG = 0 the compressive and shear curves are defined as follows: σ𝑐(𝜀𝑝𝑐, 𝜀̇𝑝𝑐), 𝜀𝑝𝑐 = 𝜀𝑐 − σ𝑠(𝛾𝑝𝑠, 𝛾̇𝑝𝑠), 𝛾𝑝𝑠 = 𝛾𝑠 − 𝜎𝑐 𝜎𝑠 , 𝜀̇𝑝𝑐 = , 𝛾̇𝑝𝑠 = 𝜕𝜀𝑝𝑐 𝜕𝑡 𝜕𝛾𝑝𝑠 𝜕𝑡 and two new history variables (#16 plastic strain in compression and #17 plastic strain in shear) are stored in addition to those history variables already stored in MAT_224. If IFLAG = 1 the compressive and shear curves are defined as follows: σ𝑐(𝜆̇, 𝜆), 𝜎𝑠(𝜆̇, 𝜆), 𝑊𝑝̇ = 𝜎eff𝜆̇ History variables may be post-processed through additional variables. The number of additional variables for solids written to the d3plot and d3thdt databases is input by the optional *DATABASE_EXTENT_BINARY card as variable NEIPH. The relevant additional variables of this material model are tabulated below: LS-PrePost history variable # 5 8 9 10 11 12 13 14 16 17 Solid elements plastic strain rate plastic failure strain triaxiality Lode parameter plastic work damage element size temperature plastic strain in compression plastic strain in shear *MAT_VISCOPLASTIC_MIXED_HARDENING This is Material Type 225. An elasto-viscoplastic material with an arbitrary stress versus strain curve and arbitrary strain rate dependency can be defined. Kinematic, isotropic, or a combination of kinematic and isotropic hardening can be specified. Also, failure based on plastic strain can be defined. Card 1 1 Variable MID 2 RO Type A8 F 3 E F 4 PR F 5 6 7 8 LCSS BETA I F Default none none none none none 0.0 Card 2 1 2 3 4 5 6 7 8 Variable FAIL Type F Default 1.0E+20 VARIABLE DESCRIPTION MID RO E PR Material identification. A unique number or label not exceeding 8 characters must be specified. Mass density. Young’s modulus. Poisson’s ratio. VARIABLE LCSS DESCRIPTION Load curve ID or Table ID. Load curve ID defining effective stress versus effective plastic strain The table ID defines for each strain rate value a load curve ID giving the stress versus effective plastic strain for that rate, See Figure M24-1. The stress versus effective plastic strain curve for the lowest value of strain rate is used if the strain rate falls below the minimum value. Likewise, the stress versus effective plastic strain curve for the highest value of strain rate is used if the strain rate exceeds the maximum value. NOTE: The strain rate values defined in the table may be given as the natural logarithm of the strain rate. If the first stress-strain curve in the table corresponds to a negative strain rate, LS-DYNA assumes that the natural logarithm of the strain rate value is used. Since the tables are internally discretized to equally space the points, natural logarithms are necessary, for example, if the curves correspond to rates from 10.e-04 to 10.e+04. BETA Hardening parameter, 0 < BETA < 1. EQ.0.0: EQ.1.0: Pure kinematic hardening Pure isotropic hardening 0.0 < BETA < 1.0: Mixed hardening FAIL Failure flag. LT.0.0: User defined failure subroutine is called to determine failure EQ.0.0: Failure is not considered. This option is recommended if failure is not of interest since many calculations will be saved. GT.0.0: Plastic strain to failure. When the plastic strain reachesthis value, the element is deleted from the cal- culation.. *MAT_KINEMATIC_HARDENING_BARLAT89_{OPTION} This is Material Type 226. This model combines Yoshida non-linear kinematic hardening rule (*MAT_125) with the 3-parameter material model of Barlat and Lian [1989] (*MAT_36) to model metal sheets under cyclic plasticity loading and with anisotropy in plane stress condition. Lankford parameters are used for the definition of the anisotropy. Yoshida’s theory describes the hardening rule with ‘two surfaces’ method: the yield surface and the bounding surface. In the forming process, the yield surface does not change in size, but its center moves with deformation; the bounding surface changes both in size and location. Available options include: <BLANK> NLP The NLP option estimates failure using the Formability Index (F.I.), which accounts for the non-linear strain paths seen in metal forming applications . When the NLP option is invoked, the variable IFLD must be specified. Additionally, the option NLP is also available in *MAT_036, *MAT_037 and *MAT_125. Card 1 1 Variable MID Type I 2 RO F 3 E F 4 PR F 5 M F 6 7 8 R00 R45 R90 F F F Default none 0.0 0.0 0.0 0.0 0.0 0.0 none Card 2 Variable 1 CB Type F 2 Y F 3 SC F 4 K F 5 RSAT F 6 SB F 7 H F 8 HLCID I Default 0.0 0.0 0.0 0.0 0.0 0.0 0.0 none Card 3 1 2 Variable AOPT IOPT Type F I 3 C1 F 4 C2 F 5 6 7 8 IFLD I Default none none 0.0 0.0 none Card 4 Variable 1 XP Type F 2 YP F 3 ZP F 4 A1 F 5 A2 F 6 A3 F 7 8 Default none none none none none none Card 5 Variable 1 V1 Type F 2 V2 F 3 V3 F 4 D1 F 5 D2 F 6 D3 F 7 8 BETA F Default none none none none none none none VARIABLE DESCRIPTION MID Material identification. A unique number must be specified. RO E PR M R00 R45 Mass density. Young’s modulus, E. Poisson’s ratio, ν. m, the exponent in Barlat’s yield criterion. 𝑅00, Lankford parameter in 0 degree direction. 𝑅45, Lankford parameter in 45 degree direction. R90 CB Y SC K *MAT_KINEMATIC_HARDENING_BARLAT89 DESCRIPTION 𝑅90, Lankford parameter in 90 degree direction. The uppercase 𝐵 defined in the Yoshida’s equations. Hardening parameter as defined in the Yoshida’s equations. The lowercase 𝑐 defined in the Yoshida’s equations. Hardening parameter as defined in the Yoshida’s equations. RSAT Hardening parameter as defined in the Yoshida’s equations. SB H HLCID The lowercase 𝑏 as defined in the Yoshida’s equations. Anisotropic parameter stagnation, defined in the Yoshida’s equations. associated with work-hardening Load curve ID in keyword *DEFINE_CURVE, where true strain and true stress relationship is characterized. The load curve is optional, and is used for error calculation only. IOPT Kinematic hardening rule flag: EQ.0: Original Yoshida formulation, EQ.1: Modified formulation: define C1, C2 as below. C1, C2 Constants used to modify 𝑅: 𝑅 = RSAT × [(𝐶1 + 𝜀̅𝑝)𝑐2 − 𝐶1 𝑐2] IFLD ID of a load curve of the traditional Forming Limit Diagram (FLD) for the linear strain paths. In the load curve, abscissas represent minor strains while ordinates represent major strains. Define only when the NLP option is used. See the example in the remarks section. AOPT Material axes option : EQ.0.0: locally orthotropic with material axes determined by element nodes 1, 2, and 4, as with *DEFINE_COORDI- NATE_NODES, and then rotated about the shell ele- ment normal by theangle BETA. EQ.2.0: globally orthotropic with material axes determined by vectors defined below, as with *DEFINE_COORDI- VARIABLE DESCRIPTION NATE_VECTOR: EQ.3.0: locally orthotropic material axes determined by rotating the material axes about the element normal by an angle, BETA, from a line in the plane of the element defined by the cross product of the vector v with the element normal: LT.0.0: the absolute value of AOPT is a coordinate system ID number (CID on *DEFINE_COORDINATE_NODES, *DEFINE_COORDINATE_SYSTEM or *DEFINE__CO- ORDINATE_VECTOR):Available with the R3 release of Version 971 and later. XP, YP, ZP Coordinates of point 𝐩 for AOPT = 1. A1, A2, A3 Components of vector 𝐚 for AOPT = 2. V1, V2, V3 Components of vector 𝐯 for AOPT = 3. D1, D2, D3 Components of vector 𝐝 for AOPT = 2. BETA Material angle in degrees for AOPT = 0 and 3, may be overridden on the element card, see *ELEMENT_SHELL_BETA. On Barlat and Lian’s yield criteron: The 𝑅-values are defined as the ratio of instantaneous width change to instantaneous thickness change. That is, assume that the width 𝑊 and thickness 𝑇 are measured as function of strain. Then the corresponding 𝑅-value is given by: 𝑅 = 𝑑𝑊 𝑑𝜀 𝑑𝑇 𝑑𝜀 /𝑊 /𝑇 Input R00, R45 and R90 to define sheet anisotropy in the rolling, 45 degree and 90 degree direction. Barlat and Lian’s [1989] anisotropic yield criterion Φ for plane stress is defined as: 𝑚 Φ = 𝑎|𝐾1 + 𝐾2|𝑚 + 𝑎|𝐾1 − 𝐾2|𝑚 + 𝑐|2𝐾2|𝑚 = 2𝜎𝑌 for face centered cubic (FCC) materials exponent m = 8 is recommended and for body centered cubic (BCC) materials m = 6 may be used. Detailed description on the criterion can be found in *MAT_036 manual pages. On Yoshida nonlinear kinematic hardening model: Background. The Yoshida’s model accounts for cyclic plasticity including Bauschinger effect and cyclic hardening behavior. For detailed Yoshida’s theory of nonlinear kinematic hardening rule and definitions of material constants CB, Y, SC, K, RSAT, SB, and H, refer to Remarks in *MAT_125 manual pages and in the original paper, “A model of large-strain cyclic plasticity describing the Baushinger effect and workhardening stagnation”, by Yoshida, F. and Uemori, T., Int. J. Plasticity, vol. 18, 661-689, 2002. Further improvements in the original Yoshida’s model, as described in a paper “Determination of Nonlinear Isotropic/Kinematic Hardening Constitutive Parameter for AHSS using Tension and Compression Tests”, by Shi, M.F., Zhu, X.H., Xia, C., and Stoughton, T., in NUMISHEET 2008 proceedings, 137-142, 2008, included modifications to allow work hardening in large strain deformation region, avoiding the problem of earlier saturation, especially for Advanced High Strength Steel (AHSS). These types of steels exhibit continuous strain hardening behavior and a non-saturated isotropic hardening function. As described in the paper, the evolution equation for R (a part of the current radius of the bounding surface in deviatoric stress space), as is with the saturation type of isotropic hardening rule proposed in the original Yoshida model, is modified as, 𝑅̇ = 𝑚(𝑅sat − 𝑅)𝑝̇ 𝑅 = RSAT × [(𝐶1 + 𝜀̅𝑝)𝑐2 − 𝐶1 𝑐2] For saturation type of isotropic hardening rule, set IOPT = 0, applicable to most of Aluminum sheet materials. In addition, the paper provides detailed variables used for this material model for DDQ, HSLA, DP600, DP780 and DP980 materials. Since the symbols used in the paper are different from what are used here, the following table provides a reference between symbols used in the paper and variables here in this keyword: B CB Y Y C SC m K K Rsat b SB h H e0 C1 N C2 b: R90 For shells, define vector a, so, c = n b = c × a a = b × c a: rolling direction R00 v × n For shells, define vector v, so, c = n a = v × n b = n × a AOPT = 2 AOPT = 3 Figure M226-1. Defining sheet metal rolling direction. Using the modified formulation and the material properties provided by the paper, the predicted and tested results compare very well both in a full cycle tension and compression test and in a pre-strained tension and compression test, according to the paper. A set of experiments are required to fit (optimize) the Yoshida material constants, and these experiments include a uniaxial tension test (used for HLCID) to a sufficiently large strain range, a full cycle tension and compression test and a multiple cycle tension and compression test. Defining the rolling direction of a sheet metal. The variable AOPT is used to define the rolling direction of the sheet metals. For shells, AOPT of 2 or 3 are relevant. When AOPT = 2, define vector components of a in the direction of the rolling (R00); when AOPT = 3, define vector components of v perpendicular to the rolling direction, as shown in Figure M226-1. Application. Application of the modified Yoshida’s hardening rule in the metal forming industry has shown significant improvement in springback prediction accuracy, which is a pre- requisite for a successful stamping tool compensation, especially for AHSS type of sheet materials. Figure M226-2. The NUMISHEET 2005 cross member and section definition. In an example shown in Figure M226-2, springback simulation was performed following drawing and trimming on the NUMISHEET 2005 cross member for aluminum alloy AL5182-O, using *MAT_226. In Figure M226-3, springback shape was recovered from section A-A (Figure M226-2), and compared with those results from simulation using *MAT_037 and *MAT_125. Though all are remarkably close, results with *MAT_226 on the cross section (Y = -370 mm) show better springback correlation to the measured test data than those with *MAT_125 and *MAT_37. To improve convergence, it is recommended that *CONTROL_IMPLICIT_FORMING type ‘1’ be used when conducting springback simulation. A Failure Criterion for Nonlinear Strain Paths (NLP): The NLP failure criterion and corresponding post processing procedures are described in the entries for *MAT_036 and *MAT_037. The history variables for every element stored in d3plot files include: 1. Formability Index (F.I.): #1 2. Strain ratio (in-plane minor strain/major strain): #2 3. Effective strain from the planar isotropic assumption: #3 The entire time history can be plotted using Post/History menu in LS-PrePost v4.0. To enable the output of these history variables to the d3plot files, NEIPS on the *DATA- BASE_EXTENT_BINARY card must be set to at least 3. When plotting the formability index, first select the history var #1 from the Misc in the FriComp menu. The pull-down menu under FriComp can be used to select minimum value ‘Min’ for necking failure determination (refer to Tharrett and Stoughton’s paper in 2003 SAE 2003-01-1157). In FriRang, the option None is to be selected in the pull-down menu next to Avg. Lastly, set the simulation result to the last state in the animation tool bar. The index value ranges from 0.0 to 1.5. The non-linear forming limit is reached when the index reaches 1.0. A partial keyword example is listed below when the option NLP is used. In this example, the traditional Forming Limit Diagram (FLD) which handles only the linear strain paths is defined by load curve ID 213. *MAT_KINEMATIC_HARDENING_BARLAT89_NLP $# mid ro e pr m r00 r45 r90 1 2.8900E-9 7.0E+4 0.333 8.0 0.699 0.776 0.775 $# cb y sc k rsat sb h hlcid 122.3 110.2 577.5 12.0 201.7 16.5 0.16 0 $# aopt iopt c1 c2 IFLD 2 0 213 $# xp yp zp a1 a2 a3 0.000 0.000 0.000 1.000000 0.000 0.000 $# v1 v2 v3 d1 d2 d3 beta 0.000 0.000 0.000 0.000 0.000 0.000 0.000 *DEFINE_CURVE 213 -0.300,0.36 -0.200,0.32 -0.114,0.266 -0.058,0.223 0.026,0.181 0.036,0.181 0.111,0.211 0.147,0.23 0.215,0.27 0.263,0.278 Revision information: This material model is available starting in Revision 57717. The NLP option is available starting in Revision 95599. AL5182 springback comparison among test data/M226/M125/M37 at section A-A (Y=-370mm) -100 -50 20 50 100 150 200 Experiments M226 m=8 M125 M37 1.3 mm 100 120 140 160 Figure M226-3. Springback prediction with *MAT_226 (Material properties courtesy of Ford Motor Company Research and Innovation Laboratory). *MAT_230 This is Material Type 230. This is a perfectly-matched layer (PML) material — an absorbing layer material used to simulate wave propagation in an unbounded isotropic elastic medium — and is available only for solid 8-node bricks (element type 2). This material implements the 3D version of the Basu-Chopra PML [Basu and Chopra (2003,2004), Basu (2009)]. 5 6 7 8 Card 1 Variable MID 2 RO Type A8 F 3 E F 4 PR F Default none none none none VARIABLE DESCRIPTION Material identification. A unique number or label not exceeding 8 characters must be specified. Mass density. Young’s modulus. Poisson’s ratio. MID RO E PR Remarks: 1. A layer of this material may be placed at a boundary of a bounded domain to simulate unboundedness of the domain at that boundary: the layer absorbs and attenuates waves propagating outward from the domain, without any signifi- cant reflection of the waves back into the bounded domain. The layer cannot support any static displacement. 2. It is assumed the material in the bounded domain near the layer is, or behaves like, an isotropic linear elastic material. The material properties of the layer should be set to the corresponding properties of this material. 3. The layer should form a cuboid box around the bounded domain, with the axes of the box aligned with the coordinate axes. Various faces of this box may be open, as required by the geometry of the problem, e.g., for a half-space prob- lem, the “top” of the box should be open. 4. Internally, LS-DYNA will partition the entire PML into regions which form the “faces”, “edges” and “corners” of the above cuboid box, and generate a new material for each region. This partitioning will be visible in the d3plot file. The user may safely ignore this partitioning. 5. The layer should have 5-10 elements through its depth. Typically, 5-6 elements are sufficient if the excitation source is reasonably distant from the layer, and 8- 10 elements if it is close. The size of the elements should be similar to that of elements in the bounded domain near the layer, and should be small enough to sufficiently discretize all significant wavelengths in the problem. 6. The nodes on the outer boundary of the layer should be fully constrained. 7. The stress and strain values reported by this material do not have any physical significance. *MAT_PML_ELASTIC_FLUID This is Material Type 230_FLUID. This is a perfectly-matched layer (PML) material with a pressure fluid constitutive law, to be used in a wave-absorbing layer adjacent to a fluid material (*MAT_ELASTIC_FLUID) in order to simulate wave propagation in an unbounded fluid medium. See the Remarks sections of *MAT_PML_ELASTIC (*MAT_- 230) and *MAT_ELASTIC_FLUID (*MAT_001_FLUID) for further details. 5 6 7 8 Card 1 Variable MID 2 RO Type A8 F 3 K F 4 VC F Default none none none none VARIABLE DESCRIPTION MID RO K VC Material identification. A unique number or label not exceeding 8 characters must be specified. Mass density Bulk modulus Tensor viscosity coefficient *MAT_PML_ACOUSTIC This is Material Type 231. This is a perfectly-matched layer (PML) material — an absorbing layer material used to simulate wave propagation in an unbounded acoustic medium — and can be used only with the acoustic pressure element formulation (element type 14). This material implements the 3D version of the Basu-Chopra PML for anti-plane motion [Basu and Chopra (2003,2004), Basu (2009)]. 4 5 6 7 8 Card 1 Variable MID 2 RO Type A8 F 3 C F Default none none none VARIABLE DESCRIPTION Material identification. A unique number or label not exceeding 8 characters must be specified. Mass density Sound speed MID RO C Remarks: 1. A layer of this material may be placed at a boundary of a bounded domain to simulate unboundedness of the domain at that boundary: the layer absorbs and attenuates waves propagating outward from the domain, without any signifi- cant reflection of the waves back into the bounded domain. The layer cannot support any hydrostatic pressure. 2. It is assumed the material in the bounded domain near the layer is an acoustic material. The material properties of the layer should be set to the correspond- ing properties of this material. 3. The layer should form a cuboid box around the bounded domain, with the axes of the box aligned with the coordinate axes. Various faces of this box may be open, as required by the geometry of the problem, e.g., for a half-space prob- lem, the “top” of the box should be open. 4. Internally, LS-DYNA will partition the entire PML into regions which form the “faces”, “edges” and “corners” of the above cuboid box, and generate a new material for each region. This partitioning will be visible in the d3plot file. The user may safely ignore this partitioning. 5. The layer should have 5-10 elements through its depth. Typically, 5-6 elements are sufficient if the excitation source is reasonably distant from the layer, and 8- 10 elements if it is close. The size of the elements should be similar to that of elements in the bounded domain near the layer, and should be small enough to sufficiently discretize all significant wavelengths in the problem. 6. The nodes on the outer boundary of the layer should be fully constrained. 7. The pressure values reported by this material do not have any physical significance. *MAT_BIOT_HYSTERETIC This is Material Type 232. This is a Biot linear hysteretic material, to be used for modeling the nearly-frequency-independent viscoelastic behaviour of soils subjected to cyclic loading, e.g. in soil-structure interaction analysis [Spanos and Tsavachidis (2001), Makris and Zhang (2000), Muscolini, Palmeri and Ricciardelli (2005)]. The hysteretic damping coefficient for the model is computed from a prescribed damping ratio by calibrating with an equivalent viscous damping model for a single-degree-of-freedom system. The damping increases the stiffness of the model and thus reduces the computed time-step size. Card 1 Variable MID 2 RO Type A8 F 3 E F 4 PR F 5 ZT F 6 FD F 7 8 Default none none none none 0.0 3.25 DESCRIPTION Material identification. A unique number or label not exceeding 8 characters must be specified. Mass density. Young’s modulus. Poisson’s ratio. Damping ratio Dominant excitation frequency in Hz VARIABLE MID RO E PR ZT FD Remarks: 1. The stress is computed as a function of the strain rate as 𝜎(𝑡) = ∫ 𝐶𝑅(𝑡 − 𝜏)𝜀̇(𝜏) 𝑑𝜏 where 𝐶𝑅(𝑡) = 𝐶 [1 + 2𝜂 𝐸1(𝛽𝑡)] with 𝐶 being the elastic isotropic constitutive tensor, 𝜂 the hysteretic damping factor, and 𝛽 = 2𝜋𝑓𝑑/10, where 𝑓𝑑 is the dominant excitation frequency in Hz. The function 𝐸1 is given by ∞ 𝐸1(𝑠) = ∫ e−𝜉 𝑑𝜉 For efficient implementation, this function is approximated by a 5-term Prony series as 𝐸1(𝑠) ≈ ∑ 𝑏𝑘e𝑎𝑘𝑠 𝑘=1 such that 𝑏𝑘 > 0. 2. The hysteretic damping factor 𝜂 is obtained from the prescribed damping ratio 𝜍 as 𝜂 = 𝜋𝜍/atan(10) = 2.14𝜍 by assuming that, for a single degree-of-freedom system, the energy dissipated per cycle by the hysteretic material is the same as that by a viscous damper, if the excitation frequency matches the natural frequency of the system. 3. The consistent Young’s modulus for this model is given by where 𝐸𝑐 = 𝐸 [1 + 2𝜂 𝑔] 𝑔 = ∑ 𝑏𝑘 𝑘=1 𝑎𝑘𝛽Δ𝑡𝑛 [exp(𝑎𝑘𝛽Δ𝑡𝑛) − 1] Because 𝑔 > 0, the computed element time-step size is smaller than that for the corresponding elastic element. Furthermore, the time-step size computed at any time depends on the previous time-step size. It can be demonstrated that the new computed time-step size stays within a narrow range of the previous time-step size, and for a uniform mesh, converges to a constant value. For 𝑓𝑑 = 3.25Hz and 𝜍 = 0.05, the percentage decrease in time-step size can be ex- pected to be about 12-15% for initial time-step sizes of less than 0.02 secs, and about 7-10% for initial time-step sizes larger than 0.02 secs. 4. The default value of the dominant frequency is chosen to be valid for earth- quake excitation. *MAT_CAZACU_BARLAT This is Material Type 233. This material model is for Hexagonal Closed Packet (HCP) metals and is based on the work by Cazacu et al. (2006). This model is capable of describing the yielding asymmetry between tension and compression for such materials. Moreover, a parameter fit is optional and can be used to find the material parameters that describe the experimental yield stresses. The experimental data that the user should supply consists of yield stresses for tension and compression in the 00 direction, tension in the 45 and the 90 directions, and a biaxial tension test. Available options include: <BLANK> MAGNESIUM Including MAGNESIUM invokes a material model developed by the USAMP consortium to simulate cast Magnesium under impact loading. The model includes rate effects having a tabulated failure model including equivalent plastic strain to failure as a function of stress triaxiality and effective plastic strain rate. Element erosion will occur when the number of integration points where the damage variable has reached unity reaches some specified threshold (NUMINT). Alternatively a Gurson type failure model can be activated, which requires less experimental data. The input of the hardening curve for MAT_233 requires the user to provide the evolution of the Cazacu-Barlat effective stress as a function of the energy conjugate plastic strain. With the MAGNESIUM option an alternative option for the hardening curve is available: von Mises effective stress as a function of equivalent plastic strain, which is energy conjugate to the von Mises stress. Finnally the MAGNESIUM option allows for distortional hardening by providing hardening curves as measured in tension and compression tests. This option is however incompatible with the activation of rate effects (visco-plasticity). With the MAGNESIUM option this material model is also available for solid elements. NOTE: Activating the MAGNESIUM options requires setting HR = 3 and FIT = 0.0. (Also see below) Card 1 1 Variable MID Type A8 Card 2 Variable Type 1 A F Card 3 1 Variable AOPT Type F 2 RO F 2 3 E F 3 4 PR F 4 5 HR F 5 C11 C22 C33 LCID F 2 F 3 I 5 6 P1 F 6 E0 F 6 7 P2 F 7 K F 7 8 ITER F 8 P3 F 8 F 4 4 A1 F 4 D1 F C12 C13 C23 C44 F F 5 A2 F 5 D2 F 6 A3 F 6 D3 F F 7 F 8 7 BETA 8 FIT F I Card 4 1 2 3 Variable Type Card 5 Variable 1 V1 Type F 2 V2 F 3 V3 Magnesium Card. Additional card for MAGNESIUM keyword option. Card 6 1 2 3 4 5 6 7 8 Variable LC1ID LC2ID NUMINT LCCID ICFLAG IDFLAG LC3ID EPSFG Type I I F I I I I F VARIABLE DESCRIPTION MID RO E PR HR Material Identification number. Constant Mass density. Young’s modulus E.GT.0.0: constant value E.LT.0.0: load curve ID (–E) which defines the Young’s modulus as a function of plastic strain. Poisson’s ratio Hardening rules: HR.EQ.1.0: linear hardening (default) HR.EQ.2.0: exponential hardening (Swift) HR.EQ.3.0: load curve HR.EQ.4.0: exponential hardening (Voce) HR.EQ.5.0: exponential hardening (Gosh) HR.EQ.6.0: exponential hardening (Hocken-Sherby) HR must be set to 3 if the MAGNESIUM option is active P1 Material parameter: HR.EQ.1.0: tangent modulus HR.EQ.2.0: 𝑞, coefficient for exponential hardening law (Swift) HR.EQ.4.0: 𝑎, coefficient for exponential hardening law (Voce) HR.EQ.5.0: 𝑞, coefficient for exponential hardening law (Gosh) HR.EQ.6.0: 𝑎, coefficient for exponential hardening law (Hocket-Sherby) VARIABLE DESCRIPTION P2 Material parameter: HR.EQ.1.0: yield stress for the linear hardening law HR.EQ.2.0: 𝑛, coefficient for (Swift) exponential hardening HR.EQ.4.0: 𝑐, coefficient for exponential hardening law (Voce) HR.EQ.5.0: 𝑛, coefficient for exponential hardening law (Gosh) HR.EQ.6.0: 𝑐, coefficient for exponential hardening law (Hocket-Sherby) ITER Iteration flag for speed: ITER.EQ.0.0: fully iterative ITER.EQ.1.0: fixed at three iterations. Generally, ITER = 0.0 is recommended. However, ITER = 1.0 is faster and may give acceptable results in most problems. A C11 Exponent in Cazacu-Barlat’s orthotropic yield surface (A > 1) Material parameter : FIT.EQ.1.0 or EQ.2.0: yield stress for tension in the 00 direction FIT.EQ.0.0: material parameter 𝑐11 C22 Material parameter : FIT.EQ.1.0 or EQ.2.0: yield stress for tension in the 45 direction FIT.EQ.0.0: material parameter 𝑐22 C33 Material parameter : FIT.EQ.1.0 or EQ.2.0: yield stress for tension in the 90 direction FIT.EQ.0.0: material parameter 𝑐33 LCID Load curve ID for the hardening law (HR.EQ.3.0), Table ID for rate dependent hardening if the MAGNESIUM option is active *MAT_CAZACU_BARLAT DESCRIPTION E0 Material parameter: HR.EQ.2.0: 𝜀0, initial yield strain for exponential hardening law (Swift) (default = 0.0) HR.EQ.4.0: 𝑏, coefficient for exponential hardening (Voce) HR.EQ.5.0: 𝜀0, initial yield strain for exponential hardening (Gosh), Default = 0.0 HR.EQ.6.0: 𝑏, coefficient for exponential hardening law (Hocket-Sherby) K Material parameter : FIT.EQ.1.0 or EQ.2.0: yield stress for compression in the 00 direction FIT.EQ.0.0: material parameter (-1 < k<1) P3 Material parameter: HR.EQ.5.0: 𝑝, coefficient for exponential hardening (Gosh) HR.EQ.6.0: 𝑛, exponent for exponential hardening law (Hocket-Sherby VARIABLE AOPT DESCRIPTION Material axes option . AOPT.EQ.0.0: locally orthotropic with material axes determined by element nodes 1, 2 and 4, as with *DEFINE_COORDINATE_NODES, and then ro- tated about the shell element normal by the an- gle BETA. AOPT.EQ.2.0: globally orthotropic with material axes determined by vectors defined below, as with *DEFINED_COORDINATE_VECTOR. AOPT.EQ.3.0: locally orthotropic material axes determined by rotating the material axes about the element normal by an angle BETA, from a line in the plane of the element defined by the cross prod- uct of the vector V with the element normal. AOPT.LT.0.0: the absolute value of AOPT is coordinate system ID (CID on *DEFINE_COORDINATE_NODES, *DE- *DEFINE_COORDINATE_SYSTEM, or FINE_COORDINATE_VECTOR). Available with the R3 release of 971 and later. Material parameter. If parameter identification (FIT = 1.0) is turned on C12 is not used. Material parameter. If parameter identification (FIT = 1.0) is turned on C13 = 0.0 Material parameter. If parameter identification (FIT = 1.0) is turned on C23 = 0.0 Material parameter FIT.EQ.1.0 or EQ.2.0: yield stress for the balanced biaxial tension test. FIT.EQ.0.0: material parameter c44 C12 C13 C23 C44 A1 - A3 Components of vector 𝐚 for AOPT = 2.0 V1 - V3 Components of vector 𝐯 for AOPT = 3.0 D1 - D3 Components of vector 𝐝 for AOPT = 2.0 BETA *MAT_CAZACU_BARLAT DESCRIPTION Material angle in degrees for AOPT = 0 and 3. NOTE, may be overridden on the element card, see *ELEMENT_SHELL_BETA FIT Flag for parameter identification algorithm: FIT.EQ.0.0: No parameter identification routine is used. The variables K, C11, C22, C33, C44, C12, C13 and C23 are interpreted as material parameters. FIT MUST be set to zero if MAGNESIUM option is active FIT.EQ.1.0: Parameter fit is used. The variables C11, C22, C33, C44 and K are interpreted as yield stresses in the 00, 45, 90 degree directions, the balanced biaxial tension and the 00 degree compression, respective- ly. It is recommended to always check the d3hsp file to see the fitted parameters before complex jobs are submitted. FIT.EQ.2.0: Same as EQ.1.0 but also produce contour plots of the yield surface. For each material three LS- PrePost ready xy-data files are created; Con- tour1_𝑛, Contour2_𝑛 and Contour3_𝑛 where 𝑛 equal the material number. Load curve ID giving equivalent plastic strain to failure as a function of stress triaxiality or a table ID giving plastic strain to failure as a function of Lode parameter and stress triaxiality (solids) Load curve ID giving equivalent plastic strain to failure as a function of equivalent plastic strain rate, the failure strain will be computed as the product of the values on LC1ID and LC2ID Number of through thickness integration points which must fail before the element is deleted (inactive for solid elements) Load curve ID giving effective stress in function of plastic strain obtained from a compression stress, input of this load curve will activate distortional hardening and is NOT compatible with the use of strain rate effects LC1ID LC2ID NUMINT LCCID DESCRIPTION Automated input conversion flag. If ICFLAG = 0 then the load curves provided under LCID and LCCID contain Cazacu-Barlat effective stress as a function of energy conjugate plastic strain. If ICFLAG = 1 then both load curves are given in terms of von Mises stress versus equivalent plastic strain Damage flag. If IDFLAG = 0 the failure model is of the Johnson Cook type and requires LC1ID and LC2ID as additional input. If IDFLAG = 1 the failure model is of the Gurson type and requires LC3ID and EPSFG as additional input Load curve giving the critical void fraction of the Gurson model as a function of the plastic strain to failure measured in the uniaxial tensile test Plastic strain to failure measured in the uniaxial tensile test, this value is used by the Gurson type failure model only. VARIABLE ICFLAG IDFLAG LC3ID EPSFG Remarks: The material model #233 (MAT_CAZACU_BARLAT) is aimed for modeling materials with strength differential and orthotropic behavior under plane stress. The yield condition includes a parameter 𝑘 that describes the asymmetry between yield in tension and compression. Moreover, to include the anisotropic behavior the stress deviator 𝐒 undergoes a linear transformation. The principal values of the Cauchy stress deviator are substituted with the principal values of the transformed tensor 𝐙, which is represented as a vector field, defined as: where nents𝑆𝐼 = (𝑠11, 𝑠22, 𝑠33, 𝑠12), the 𝐒is field 𝐙 = 𝐂𝐒 (233.1) comprised of the four stresses deviator 𝐬 = σ − tr(σ)δ, where tr(σ) is the trace of the Cauchy stress tensor and δ is the Kronecker delta. For the 2D plane stress condition, the orthotropic condition gives 7 independent coefficients. The tensor 𝐂 is represented by the 4𝑥4 matrix 𝐶𝐼𝐽 = 𝑐12 𝑐22 𝑐23 𝑐13 𝑐23 𝑐33 𝑐11 𝑐12 𝑐13 ⎜⎜⎜⎜⎜⎛ ⎝ ⎟⎟⎟⎟⎟⎞ . 𝑐44⎠ The principal values of 𝐙 are denoted Σ1, Σ2, Σ3 and are given as the eigenvalues to the matrix composed by the components Σ𝑥𝑥, Σ𝑦𝑦, Σ𝑧𝑧, Σ𝑥𝑦through where Σ1 = Σ2 = (Σ𝑥𝑥 + Σ𝑦𝑦 + √(Σ𝑥𝑥 − Σ𝑦𝑦) + 4Σ𝑥𝑦 2 ) , (Σ𝑥𝑥 + Σ𝑦𝑦 − √(Σ𝑥𝑥 − Σ𝑦𝑦) + 4Σ𝑥𝑦 2 ) , Σ3 = Σ𝑧𝑧 3Σ𝑥𝑥 = (2𝑐11 − 𝑐12 − 𝑐13)𝜎𝑥𝑥 + (−𝑐11 + 2𝑐12 − 𝑐13)𝜎𝑦𝑦, 3Σ𝑦𝑦 = (2𝑐12 − 𝑐22 − 𝑐23)𝜎𝑥𝑥 + (−𝑐12 + 2𝑐22 − 𝑐23)𝜎𝑦𝑦, 3Σ𝑧𝑧 = (2𝑐13 − 𝑐23 − 𝑐33)𝜎𝑥𝑥 + (−𝑐13 + 2𝑐23 − 𝑐33)𝜎𝑦𝑦, Σ𝑥𝑦 = 𝑐44𝜎12 Note that the symmetry of Σ𝑥𝑦 follows from the symmetry of the Cauchy stress tensor. The yield condition is written on the following form: 𝑓 (Σ, 𝑘, 𝜀ep) = 𝜎eff(Σ1, Σ2, Σ3, 𝑘) − 𝜎𝑦(𝜀ep) ≤ 0 (233.2) where 𝜎𝑦(𝜀ep) is a function representing the current yield stress dependent on current effective plastic strain and 𝑘 is the asymmetric parameter for yield in compression and tension. The effective stress 𝜎effis given by 𝜎eff = [(|Σ1| − 𝑘Σ1)𝑎 + (|Σ2| − 𝑘Σ2)𝑎 + (∣Σ3∣ − 𝑘Σ3)𝑎] 𝐶 represent the yield stress along the rolling 𝑇 and 𝜎00 where 𝑘 ∈ [−1,1], 𝑎 ≥ 1. Now, let 𝜎00 𝑇 and (00 degree) direction in tension and compression, respectively. Furthermore let 𝜎45 𝑇 be 𝑇 represent the yield stresses in the 45 and the 90 degree directions, and last let 𝜎𝐵 𝜎90 the balanced biaxial yield stress in tension. Following Cazacu et al. (2006) the yield stresses can easily be derived. (233.3) 𝑎⁄ To simplify the equations it is preferable to make the following definitions: Φ1 = Φ2 = Φ3 = (2𝑐11 − 𝑐12 − 𝑐13) Ψ1 = (2𝑐12 − 𝑐22 − 𝑐23) and Ψ2 = (2𝑐13 − 𝑐23 − 𝑐33) Ψ3 = (−𝑐11 + 2𝑐12 − 𝑐13) (−𝑐12 + 2𝑐22 − 𝑐23) (−𝑐13 + 2𝑐23 − 𝑐33) The yield stresses can now be written as: 1. In the 00 degree direction: 𝑇 = [ 𝜎00 𝐶 = [ 𝜎00 (𝜎eff)𝑎 (|Φ1| − 𝑘Φ1)𝑎 + (|Φ2| − 𝑘Φ2)𝑎 + (∣Φ3∣ − 𝑘Φ3)𝑎] (𝜎eff)𝑎 (|Φ1| + 𝑘Φ1)𝑎 + (|Φ2| + 𝑘Φ2)𝑎 + (∣Φ3∣ + 𝑘Φ3)𝑎] 𝑎⁄ , 𝑎⁄ 2. In the 45 degree direction: 𝑇 = [ 𝜎45 (𝜎eff)𝑎 (|Λ1| − 𝑘Λ1)𝑎 + (|Λ2| − 𝑘Λ2)𝑎 + (∣Λ3∣ − 𝑘Λ3)𝑎] 𝑎⁄ where Λ1 = Λ2 = Λ3 = [Φ1 + Φ2 + Ψ1 + Ψ2 + √(Φ1 + Ψ1 − Φ2 − Ψ2)2 + 4𝑐44 2 ] , [Φ1 + Φ2 + Ψ1 + Ψ2 − √(Φ1 + Ψ1 − Φ2 − Ψ2)2 + 4𝑐44 2 ] , [Φ3 + Ψ3]. 3. In the 90 degree direction: 𝑇 = [ 𝜎90 (𝜎eff)𝑎 (|Ψ1| − 𝑘Ψ1)𝑎 + (|Ψ2| − 𝑘Ψ2)𝑎 + (∣Ψ3∣ − 𝑘Ψ3)𝑎] 𝑎⁄ 4. In the balanced biaxial yield occurs when both 𝜎𝑥𝑥 and 𝜎𝑦𝑦are equal to: 𝑇 = [ 𝜎𝐵 (𝜎eff)𝑎 (|Ω1| − 𝑘Ω1)𝑎 + (|Ω2| − 𝑘Ω2)𝑎 + (∣Ω3∣ − 𝑘Ω3)𝑎] 𝑎⁄ where (233.4) (233.5) (233.6) (233.7) Ω1 = Ω2 = Ω3 = (𝑐11 + 𝑐12 − 2𝑐13) (𝑐12 + 𝑐22 − 2𝑐23) (𝑐13 + 𝑐23 − 2𝑐33) Hardening laws: The implemented hardening laws are the following: 1. The Swift hardening law 2. The Voce hardening law 3. The Gosh hardening law 4. The Hocket-Sherby hardening law 5. A loading curve, where the yield stress is given as a function of the effective plastic strain The Swift’s hardening law can be written where 𝑞 and 𝑛 are material parameters. 𝜎𝑦(𝜀ep) = 𝑞(𝜀0 + 𝜀ep) The Voce’s equation says that the yield stress can be written in the following form 𝜎𝑦(𝜀ep) = 𝑎 − 𝑏𝑒−𝑐𝜀ep where 𝑎, 𝑏and 𝑐 are material parameters. The Gosh’s equation is similar to Swift’s equation. They only differ by a constant 𝜎𝑦(𝜀ep) = 𝑞(𝜀0 + 𝜀ep) − 𝑝 where 𝑞, 𝜀0, 𝑛 and 𝑝 are material constants. The Hocket-Sherby equation resemblance the Voce’s equation, but with an additional parameter added 𝜎𝑦(𝜀ep) = 𝑎 − 𝑏𝑒−𝑐𝜀ep where 𝑎, 𝑏, 𝑐 and 𝑛 are material parameters. Constitutive relation and material stiffness: The classical elastic constitutive equation for linear deformations is the well-known Hooke’s law. This relation written in a rate formulation is given by 𝛔̇ = 𝐃ε̇𝑒 (233.8) where ε𝑒 is the elastic strain and 𝐃 is the constitutive matrix. An over imposed dot indicates differentiation respect to time. Introducing the total strain εand the plastic strain ε𝑝, Eq. (233.8) is classically rewritten as 𝛔̇ = 𝐃(𝜺̇ − 𝜺̇𝑝) (233.9) *MAT_233 𝐃 = 1 − 𝜈2 ⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎛1 ⎝ 1 − 𝑣 1 − 𝑣 ⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎞ 1 − 𝑣 2 ⎠ and (ε̇ − ε̇𝑝) = ⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎛ ⎝ 11 𝜀̇11 − (𝜀̇𝑝) 𝜀̇22 − (𝜀̇𝑝) 22 2[𝜀̇12 − (𝜀̇𝑝) 12 2[𝜀̇13 − (𝜀̇𝑝) 13 2[𝜀̇23 − (𝜀̇𝑝) 23 ⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎞ ] ] ]⎠ . The parameters 𝐸and 𝑣 are the Young’s modulus and Poisson’s ratio, respectively. The material stiffness 𝐃𝑝 that is needed for e.g., implicit analysis can be calculated from (233.9) as 𝐃𝑝 = ∂𝛔̇ ∂ε̇ . The associative flow rule for the plastic strain is usually written and the consistency condition reads ε̇𝑝 = 𝜆̇ ∂𝑓 ∂𝛔 d𝑓 d𝛔 𝛔̇ + d𝑓 dεep ε̇ep = 0. (233.10) (233.10) (233.11) Note that the centralized “dot” means scalar product between two vectors. Using standard calculus one easily derives from (1.9), (1.10) and (1.11) an expression for the stress rate 𝛔̇ = 𝐃 − ⎡ ⎢ ⎢ ⎢ ⎢ ⎣ (𝐃 d𝑓 d𝛔 ) ⋅ (𝐃 𝑑𝑓 𝑑𝛔 ⋅ (𝐃 d𝑓 d𝛔 ) − ) d𝑓 ⎤ ⎥ d𝝈 ⎥ ⎥ d𝑓 ⎥ dε𝑒𝑝⎦ ε̇ (233.12) That means that the material stiffness used for implicit analysis is given by 𝐃𝑝 = 𝐃 − (𝐃 d𝑓 d𝛔 ) ⋅ (𝐃 d𝑓 d𝛔 ⋅ (𝐃 d𝑓 d𝝈 ) − ) d𝑓 d𝛔 d𝑓 d𝜀ep . (233.13) To be able to do a stress update we need to calculate the tangent stiffness and the derivative with respect to the corresponding hardening law. When a suitable hardening law has been chosen the corresponding derivative is simple and will be left out from this document. However, the stress gradient of the yield surface is more complicated and will be outlined here. ∂𝑓 𝜕σ11 = 𝜕𝑓 𝜕Σ3 𝜕𝑓 ⎜⎛1 + ⎢⎡ 𝜕Σ1 ⎣ ⎝ Σ𝑥𝑥 − Σ𝑦𝑦 √Σ𝑇 ⎠ ⎟⎞ Φ1 + ⎜⎛1 − ⎝ Σ𝑥𝑥 − Σ𝑦𝑦 ⎟⎞ Φ2 ⎥⎤ ⎦ √Σ𝑇 ⎠ + 𝜕𝑓 ⎜⎛1 − ⎢⎡ 𝜕Σ2 ⎣ ⎝ Σ𝑥𝑥 − Σ𝑦𝑦 ⎟⎞ Φ1 + ⎜⎛1 + ⎝ √Σ𝑇 ⎠ Σ𝑥𝑥 − Σ𝑦𝑦 √Σ𝑇 ⎠ ⎟⎞ Φ2 (233.14) ⎥⎤ + Φ3 ⎦ 𝜕𝑓 𝜕𝜎22 = 𝜕𝑓 ⎜⎛1 + ⎢⎡ 𝜕Σ1 ⎣ ⎝ Σ𝑥𝑥 − Σ𝑦𝑦 ⎟⎞ Ψ1 + ⎜⎛1 − ⎝ Σ𝑥𝑥 − Σ𝑦𝑦 ⎟⎞ Ψ2 ⎥⎤ ⎦ √Σ𝑇 ⎠ √Σ𝑇 ⎠ + 𝜕𝑓 ⎜⎛1 − ⎢⎡ 𝜕Σ2 ⎣ ⎝ Σ𝑥𝑥 − Σ𝑦𝑦 ⎟⎞ Ψ1 + ⎜⎛1 + ⎝ √Σ𝑇 ⎠ Σ𝑥𝑥 − Σ𝑦𝑦 ⎟⎞ Ψ2 √Σ𝑇 ⎠ and the derivative with respect to the shear stress component is 𝜕𝑓 𝜕𝜎12 = 𝑐44 2Σ𝑥𝑦 √Σ𝑇 ( 𝜕𝑓 𝜕Σ1 − 𝜕𝑓 𝜕Σ2 ) Σ𝑇 = (Σ𝑥𝑥 − Σ𝑦𝑦) + 4Σ𝑥𝑦 where and (233.15) 𝜕𝑓 𝜕Σ3 ⎥⎤ + ⎦ Ψ3 (233.16) (233.17) 𝑎−1 = 𝑓 (Σ, 𝑘, 𝜀𝑒𝑝) 𝜕𝑓 𝜕Σ𝑖 (|Σ𝑖| − 𝑘Σ𝑖)𝑎−1(sgn(Σ𝑖) − 𝑘) for 𝑖 = 1,2,3 (233.18) Implementation: Assume that the stress and strain is known at time 𝑡𝑛. A trial stress σ̃𝑛+1 at time 𝑡𝑛+1 is calculated by assuming a pure elastic deformation, i.e., 𝛔̃𝑛+1 = 𝛔𝑛 + 𝐃(ε𝑛+1 − ε𝑛) (233.19) Now, if 𝑓 (Σ, 𝑘, 𝜀𝑒𝑝) ≤ 0 the deformation is pure elastic and the new stress and plastic strain are determined as 𝛔𝑛+1 = 𝛔̃𝑛+1 𝑛+1 = 𝜀ep 𝜀ep and the thickness strain increment is given by Δ𝜀33 = 𝜀33 𝑛+1 − 𝜀33 𝑛 = − 1 − 𝑣 (Δ𝜀11 + Δ𝜀22) (233.20) (233.21) If the deformation is not pure elastic the stress is not inside the yield surface and a plastic iterative procedure must take place. 1. Set 𝑚 = 0, 𝛔(0) 𝑛+1 = 𝛔̃𝑛+1, 𝜀ep(0) 𝑛+1 = 𝜀ep 𝑛 and Δ𝜀11 𝑝(0) = Δ𝜀22 𝑝(0) = 0 2. Determine the plastic multiplier as Δ𝜆 = d𝑓 d𝛔 𝑛+1 ) 𝑛+1, 𝜀ep(𝑚) 𝑓 (𝛔(𝑚) d𝑓 d𝛔 (σ(𝑚) 𝑛+1) ⋅ 𝐃 𝑛+1) − (σ(𝑚) d𝑓 d𝜀ep 𝑛+1 ) (𝜀ep(𝑚) (233.22) 3. Perform a plastic corrector step: 𝛔(𝑚+1) increments in plastic strain according to 𝑛+1 = 𝛔(𝑚) 𝑛+1 − Δ𝜆𝐃 𝑛+1 𝜀ep(𝑚+1) = 𝜀ep(𝑚) 𝑛+1 + Δ𝜆 Δ𝜀11 𝑝(𝑛+1) = Δ𝜀11 𝑝(𝑛) + Δ𝜆 Δ𝜀22 𝑝(𝑛+1) = Δ𝜀22 𝑝(𝑛) + Δ𝜆 ∂𝑓 𝜕𝜎11 𝜕𝑓 𝜕𝜎22 (𝜎(𝑚) 𝑛+1) (𝜎(𝑚) 𝑛+1) 4. If ∣𝑓 (σ(𝑚+1) 𝑛+1 , 𝜀ep 𝑛 )∣ < tol or 𝑚 = 𝑚max; stop and set , , 𝑛+1 𝑛+1 𝛔𝑛+1 = 𝛔(𝑚+1) 𝑛+1 = 𝜀ep(𝑚+1) 𝜀ep 𝑝 = Δ𝜀11 𝑝 = Δ𝜀22 Δ𝜀11 Δ𝜀22 𝑝(𝑚+1), 𝑝(𝑚+1), d𝑓 d𝛔 (𝛔(𝑚) 𝑛+1) and find the (233.23) (233.24) otherwise set 𝑚 = 𝑚 + 1and return to 2. The thickness strain increment is for plastic yield calculated as Δ𝜀33 = − 1 − 𝑣 (Δ𝜀11 + Δ𝜀22) − (1 − 1 − 𝑣 ) (Δ𝜀11 𝑝 ) 𝑝 + Δ𝜀22 (233.25) The following history variables will be stored for the MAGNESIUM option: HV1 HV6 HV7 HV8 HV9 equivalent plastic strain (energy conjugate to Cazacu-Barlat effective stress) damage plastic strain to failure number of IP that failed equivalent plastic strain (energy conjugate to von Mises stress) effective stress (Cazacu-Barlat) HV10 HV11 Gurson damage HV12 HV13 HV14 void fraction void fraction star equivalent plastic strain (energy conjugate to von Mises stress) *MAT_VISCOELASTIC_LOOSE_FABRIC This is Material Type 234 developed and implemented by Tabiei et al [2004]. The model is a mechanism incorporating the crimping of the fibers as well as the trellising with reorientation of the yarns and the locking phenomenon observed in loose fabric. The equilibrium of the mechanism allows the straightening of the fibers depending on the fiber tension. The contact force at the fiber cross over point determines the rotational friction dissipating a part of the impact energy. The stress-strain relationship is viscoelastic based on a three-element model. The failure of the fibers is strain rate dependent. *DAMPING_PART_MASS is recommended to be used in conjunction with this material model. This material is valid for modeling the elastic and viscoelastic response of loose fabric used in body armor, blade containments, and airbags. fill yarn warp yarn Figure M234-1. Representative Volume Cell (RVC) of the model Card 1 1 Variable MID Type A8 Card 2 Variable 1 TA Type F 2 RO F 2 W F 3 E1 F 3 s F 4 E2 F 4 T F 5 G12 F 5 H F 6 EU F 6 S F 7 THL F 7 8 THI F 8 EKA EUA F 4 5 6 7 8 G23 EKB AOPT *MAT_234 Card 3 1 Variable VMB Type F Card 4 1 2 C F 2 F 3 F 4 Variable Not used Not used Not used A1 Type Card 5 Variable 1 V1 Type F 2 V2 F 3 V3 F F 4 D1 F F 5 A2 F 5 D2 F 6 A3 F 6 D3 F 7 8 7 8 VARIABLE DESCRIPTION MID RO E1 E2 G12 EU THL THI TA W Material identification. A unique number or label not exceeding 8 characters must be specified. Mass density. 𝐸1, Young’s modulus in the yarn axial-direction. 𝐸2, Young’s modulus in the yarn transverse-direction. 𝐺12, Shear modulus of the yarns. Ultimate strain at failure. Yarn locking angle. Initial braid angle. Transition angle to locking. Fiber width. VARIABLE DESCRIPTION S T H S EKA EUA VMB C G23 Ekb AOPT Span between the fibers. Real fiber thickness. Effective fiber thickness. Fiber cross-sectional area. Elastic constant of element "a". Ultimate strain of element "a". Damping coefficient of element "b". Coefficient of friction between the fibers. transverse shear modulus. Elastic constant of element "b" Material axes option . AOPT.EQ.0.0: locally orthotropic with material axes determined by element nodes 1, 2 and 4, as with *DEFINE_COORDINATE_NODES. AOPT.EQ.2.0: globally orthotropic with material axes determined by vectors defined below, as with *DEFINED_COORDINATE_VECTOR. AOPT.EQ.3.0: locally orthotropic material axes defined by the cross product of the vector V with the element normal. AOPT.LT.0.0: the absolute value of AOPT is coordinate system ID (CID on *DEFINE_COORDINATE_NODES, *DEFINE_COORDINATE_SYSTEM, or *DE- FINE_COORDINATE_VECTOR). Available with the R3 release of 971 and later. 45o 45o a) b) min min c) Figure M234-2. Plain woven fabric as trellis mechanism: a) initial state; b) slightly stretched in bias direction; c) stretched to locking. Remarks: The parameters of the Representative Volume Cell (RVC) are: the yarn span, s, the fabric thickness, t, the yarn width, w, and the yarn cross-sectional area, 𝐴. The initially orthogonal yarns are free to rotate up to some angle and after that the lateral contact between the yarns causes the locking of the trellis mechanism and the packing of the yarns .The minimum braid angle, 𝜃min, can be calculated from the geometry and the architecture of the fabric material having the yarn width, 𝑤, and the span between the yarns, 𝑠: sin(2𝜃min) = The other constrain angles as the locking range angle, 𝜃lock, and the maximum braid angle, 𝜃max, are easy to be determined then: 𝜃𝑙𝑜𝑐𝑘 = 45° − 𝜃min , 𝜃max = 45° + 𝜃lock The material behavior of the yarn can be simply described by a combination of one Maxwell element without the dashpot and one Kelvin-Voigt element. The 1-D model of viscoelasticity is shown in the following figure. The differential equation of viscoelasticity of the yarns can be derived from the model equilibrium as in the following equation: (𝐾𝑎 + 𝐾𝑏)𝜎 + 𝜇𝑏𝜎̇ = 𝐾𝑎𝐾𝑏𝜀 + 𝜇𝑏𝐾𝑎𝜀̇ σ, ε Ka σ , ε σ , ε Kb σ, ε Figure M234-3. Three-element visvoelasticity model The input parameters for the viscoelasticity model of the material are only the static Young’s modulus E1, the Hookian spring coefficient (EKA) 𝐾𝑎, the viscosity coefficient (VMB) 𝜇𝑏, the static ultimate strain (EU) 𝜀max, and the Hookian spring ultimate strain (EUA)𝜀𝑎max. The other parameters can be obtained as follows: 𝐾𝑏 = 𝜀𝑏max = 𝐾𝑎𝐸1 𝐾𝑎 − 𝐸1 𝐾𝑎 − 𝐸1 𝐾𝑎 𝜀max Applying the Eq. (18) for the fill and the warp yarns, we obtain the stress increments in the yarns, Δ𝜎𝑓 and Δ𝜎𝑤,. The stress in the yarns is updated for the next time step: (𝑛), (𝑛) (𝑛+1) = 𝜎𝑤 𝜎𝑤 (𝑛) + Δ𝜎𝑤 (𝑛+1) = 𝜎𝑓 𝜎𝑓 (𝑛) + Δ𝜎𝑓 We can imagine that the RVC is smeared to the parallelepiped in order to transform the stress acting on the yarn cross-section to the stress acting on the element wall. The thickness of the membrane shell element used should be equal to the effective thickness, 𝑡𝑒, that can be found by dividing the areal density of the fabric by its mass density. The in-plane stress components acting on the RVC walls in the material direction of the yarns are calculated as follows for the fill and warp directions: (𝑛+1)𝑆 2𝜎𝑓 (𝑛+1) = 𝜎𝑓11 𝑠𝑡𝑒 (𝑛) + 𝛼𝐸2Δ𝜀𝑓22 (𝑛+1) = 𝜎𝑓22 𝜎𝑓22 (𝑛) (𝑛+1) = 𝜎𝑓12 𝜎𝑓12 (𝑛) + 𝛼𝐺12Δ𝜀𝑓12 (𝑛) 2𝜎𝑤 𝜎𝑤11 (𝑛+1) = (𝑛+1)𝑆 𝑠𝑡𝑒 (𝑛) + 𝛼𝐸2Δ𝜀𝑤22 (𝑛+1) = 𝜎𝑤22 𝜎𝑤22 (𝑛) (𝑛+1) = 𝜎𝑤12 𝜎𝑤12 (𝑛) + 𝛼𝐺12Δ𝜀𝑤12 (𝑛) lock lock Δθ Δθ min 45o max Figure M234-4. The lateral contact factor as a function of average braid angle θ. where E2 is the transverse Young’s modulus of the yarns, 𝐺12 is the longitudinal shear modulus, and α is the lateral contact factor. The lateral contact factor is zero when the trellis mechanism is open and unity if the mechanism is locked with full lateral contact between the yarns. There is a transition range, Δ𝜃 × TA, of the average braid angle 𝜃 in which the lateral contact factor, 𝛼, is a linear function of the average braid angle. The graph of the function 𝛼(𝜃) is shown in Fig. M234-4. *MAT_MICROMECHANICS_DRY_FABRIC This is Material Type 235 developed and implemented by Tabiei et al [2001]. The the material model derivation utilizes homogenization technique usually used in composite material models. The model accounts for reorientation of the yarns and the fabric architecture. The behavior of the flexible fabric material is achieved by discounting the shear moduli of the material in free state, which allows the simulation of the trellis mechanism before packing the yarns. This material is valid for modeling the elastic response of loose fabric used in inflatable structures, parachutes, body armor, blade containments, and airbags. the micro-mechanical approach and 2 RO F 2 3 E1 F 3 4 E2 F 4 5 6 7 8 G12 G23 V12 V23 F 5 F 6 F 7 F 8 THI THL BFI BWI DSCF CNST ATLR F 2 F 3 F 4 F 5 Variable VMB VME TRS FFLG AOPT Type F Card 4 1 F 2 F 3 F 4 Variable Not used Not used Not used A1 Type F F 5 A2 F F 7 F 8 7 8 F 6 6 A3 F Card 1 1 Variable MID Type A8 Card 2 Variable 1 XT Type F Card 3 Variable 1 V1 Type F *MAT_MICROMECHANICS_DRY_FABRIC 2 V2 F 3 V3 F 4 D1 F 5 D2 F 6 D3 F 7 8 VARIABLE DESCRIPTION MID RO E1 E2 G12 G23 V12 V23 XT THI THL BFI BWI DSCF CNST ATLR VME VMS TRS Material identification. A unique number or label not exceeding 8 characters must be specified. Mass density. 𝐸1, Young’s modulus of the yarn in axial-direction. 𝐸2, Young’s modulus of the yarn in transverse-direction. 𝐺12, shear modulus of the yarns. 𝐺23, transverse shear modulus of the yarns. Poisson’s ratio. Transverse Poisson’s ratio. Stress or strain to failure . Initial brade angle. Yarn locking angle. Initial undulation angle in fill direction. Initial undulation angle in warp direction. Discount factor Reorientation damping constant Angle tolerance for locking Viscous modulus for normal strain rate Viscous modulus for shear strain rate Transverse shear modulus of the fabric layer Figure M235-1. Yarn orientation schematic. VARIABLE DESCRIPTION FFLG Flag for stress-based or strain-based failure EQ.0: XT is a stress to failure NE.0: XT is a strain to failure AOPT Material axes option . AOPT.EQ.0.0: locally orthotropic with material axes determined by element nodes 1, 2 and 4, as with *DEFINE_COORDINATE_NODES. AOPT.EQ.2.0: globally orthotropic with material axes determined by vectors defined below, as with *DEFINED_COORDINATE_VECTOR. AOPT.EQ.3.0: locally orthotropic material axes defined by the cross product of the vector V with the element normal. AOPT.LT.0.0: the absolute value of AOPT is coordinate system ID (CID on *DEFINE_COORDINATE_NODES, *DEFINE_COORDINATE_SYSTEM, or *DE- FINE_COORDINATE_VECTOR). Available with the R3 release of 971 and later. A1 - A3 Components of vector 𝐚 for AOPT = 2.0 V1 - V3 Components of vector 𝐯 for AOPT = 3.0 D1 - D3 Components of vector 𝐝 for AOPT = 2.0 Remarks: The Representative Volume Cell (RVC) approach is utilized in the micro-mechanical model development. The direction of the yarn in each sub-cell is determined by two angles – the braid angle, 𝜃 (the initial braid angle is 45 degrees), and the undulation angle of the yarn, which is different for the fill and warp-yarns, 𝛽𝑓 and 𝛽𝑤 (the initial undulations are normal few degrees), respectively. The starting point for the homogenization of the material properties is the determination of the yarn stiffness matrices. The elasticity tensor is given by [𝐶′] = [𝑆′]−1 = 𝐸1 𝜈12 𝐸1 𝜈12 𝐸1 − − ⎡ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎣ 0 0 0 − − 𝜈12 𝐸1 𝐸2 𝜈23 𝐸2 − − 𝜈12 𝐸1 𝜈23 𝐸2 𝐸2 0 0 0 0 0 𝜇𝐺12 0 0 0 0 0 0 0 𝜇𝐺23 0 0 0 0 −1 0 0 0 ⎤ ⎥ ⎥ ⎥ ⎥ ⎥ ⎥ ⎥ ⎥ ⎥ ⎥ ⎥ ⎥ ⎥ ⎥ ⎥ ⎥ 𝜇𝐺12⎦ 0 0 where 𝐸1, 𝐸2, 𝜈12, 𝜈23, 𝐺12 and 𝐺23 are Young’s moduli, Poisson’s ratios, and the shear moduli of the yarn material, respectively. 𝜇 is a discount factor, which is function of the braid angle, 𝜃, and has value between 𝜇0 and 1 as shown in the next figure. Initially, in free stress state, the discount factor is a small value (DSCF = 𝜇0 A 1) and the material has very small resistance to shear deformation if any. 45o 45o Plain Woven Fabric: Free State Representative Volume Cell Plain Woven Fabric: Stretched min min Plain Woven Fabric: Compacted When the locking occurs, the fabric yarns are packed and they behave like elastic media. The discount factor is unity as shown in the next figure. The micro-mechanical model is developed to account for the reorientation of the yarns up to the locking angle. The locking angle, 𝜃lock, can be obtained from the yarn width and the spacing parameter of the fabric using simple geometrical relationship. The transition range, Δ𝜃 (angle tolerance for locking), can be chosen to be as small as possible, but big enough to prevent high frequency oscillations in transition to compacted state and depends on the range to the locking angle and the dynamics of the simulated problem. Reorientation damping constant is defined to damp some of the high frequency oscillations. A simple rate effect is added by defining the viscous modulus for normal or shear strain rate . (VMB*𝜀11 or 22 . for normal components and VMS*𝜀12 for the shear components). fill yarn qf qw locking area warp yarn RVC dn 45o up lock lock Locking Angles lock lock Δθ Δθ dn 45o up Discount factor as a function of braid angle, θ *MAT_236 This is Material Type 236 developed by Carney, Lee, Goldberg, and Santhanam [2007]. This model simulates silicon carbide coating on Reinforced Carbon-Carbon (RCC), a ceramic matrix and is based upon a quasi-orthotropic, linear-elastic, plane-stress model. Additional constitutive model attributes include a simple (i.e. non-damage model based) option that can model the tension crack requirement: a “stress-cutoff” in tension. This option satisfies the tension crack requirements by limiting the stress in tension but not compression, and having the tensile “yielding” (i.e. the stress-cutoff) be fully recoverable – not plasticity or damage based. Card 1 1 Variable MID Type A8 Card 2 Variable 1 PR Type F VARIABLE MID 2 RO F 2 G F 3 E0 F 3 4 E1 F 4 5 E2 F 5 6 E3 F 6 7 E4 F 7 8 E5 F 8 G_SCL TSL EPS_TAN F F F DESCRIPTION Material identification. A unique number or label not exceeding 8 characters must be specified. RO Mass density. E0 E1 E2 E3 E4 E5 E0, See Remarks below. E1, See Remarks below. E2, See Remarks below. E3, See Remarks below. E4, See Remarks below. E5, Young’s modulus of the yarn in transverse-direction. *MAT_SCC_ON_RCC DESCRIPTION PR G Poisson’s ratio. Shear modulus G_SCL Shear modulus multiplier (default = 1.0). TSL Tensile limit stress EPS_TAN Strain at which E = tangent to the polynomial curve. Remarks: This model for the silicon carbide coating on RCC is based upon a quasi-orthotropic, linear-elastic, plane-stress model, given by: {⎧𝜎1 }⎫ 𝜎2 𝜏12⎭}⎬ ⎩{⎨ = ⎡ 1 − 𝜈2 ⎢ ⎢ 𝜈𝐸 ⎢ ⎢ 1 − 𝜈2 0 ⎣ 𝜈𝐸 1 − 𝜈2 1 − 𝜈2 0 {⎧𝜀1 }⎫ 𝜀2 𝛾12⎭}⎬ ⎩{⎨ 0 ⎤ ⎥ ⎥ ⎥ ⎥ 𝐺12⎦ 0 Additional constitutive model requirements include a simple (i.e. non-damage model based) option that can model the tension crack requirement: a “stress-cutoff” in tension. This option satisfies the tension crack requirements by limiting the stress in tension but not compression, and having the tensile “yielding” (i.e. the stress-cutoff) be fully recoverable – not plasticity or damage based. The tension stress-cutoff separately resets the stress to a limit value when it is exceeded in each of the two principal directions. There is also a strain-based memory criterion that ensures unloading follows the same path as loading: the “memory criterion” is the tension stress assuming that no stress cutoffs were in effect. In this way, when the memory criterion exceeds the user-specified cutoff stress, the actual stress will be set to that value. When the element unloads and the memory criterion falls back below the stress cutoff, normal behavior resumes. Using this criterion is a simple way to ensure that unloading does not result in any hysteresis. The cutoff criterion cannot be based on an effective stress value because effective stress does not discriminate between tension and compression, and also includes shear. This means that the in plane, 1- and 2- directions must be modeled as independent to use the stress cutoff. Because the Poisson’s ratio is not zero, this assumption is not true for cracks that may arbitrarily lie along any direction. However, careful examination of damaged RCC shows that generally, the surface cracks do tend to lie in the fabric directions, meaning that cracks tend to open in the 1- or the 2- direction independently. So the assumption of directional independence for tension cracks may be appropriate for the coating because of this observed orthotropy. The quasi-orthotropic, linear-elastic, plane-stress model with tension stress cutoff (to simulate tension cracks) can model the as-fabricated coating properties, which do not show nonlinearities, but not the non-linear response of the flight-degraded material. Explicit finite element analysis (FEA) lends itself to nonlinear-elastic stress-strain relation instead of linear-elastic. Thus, instead of 𝝈 = 𝐄𝜺, the modulus will be defined as a function of some effective strain quantity, or 𝝈 = 𝐄(𝜺eff) ⋅ 𝜺, even though it is uncertain, from the available data, whether or not the coating response is completely nonlinear- elastic, and does not include some damage mechanism. This nonlinear-elastic model cannot be implemented into a closed form solution or into an implicit solver; however, for explicit FEA such as is used for LS-DYNA impact analysis, the modulus can be adjusted at each time step to a higher or lower value as desired. In order to model the desired S-shape response curve of flight-degraded RCC coating, a function of strain that replicates the desired response must be found. It is assumed that the nonlinearities in the material are recoverable (elastic) and that the modulus is communicative between the 1- and 2- directions (going against the tension- crack assumption that the two directions do not interact). Sometimes stability can be a problem for this type of nonlinearity modeling, however, stability was not found to be a problem with the material constants used for the coating. The von Mises strain is selected for the effective strain definition as it couples the 3- dimensional loading but reduces to uniaxial data, so that the desired uniaxial compressive response can be reproduced. So, 𝜀eff = √2 1 + 𝜈 2 √(𝜀1 − 𝜀2)2 + (𝜀2 − 𝜀3)2 + (𝜀1 − 𝜀3)2 + 3𝛾12 where for a 2-D, isotropic shell element case, the z-direction strain is given by: The function for modulus is implemented as an arbitrary 5th order polynomial: 𝜀3 = −𝜈 1 − 𝜈 (𝜀1 + 𝜀2) 𝐸(𝜀eff) = 𝐴0𝜀eff 5 1 + ⋯ + 𝐴5𝜀eff 0 + 𝐴1𝜀eff In the case of as-fabricated material the first coefficient (A0) is simply the modulus E, and the other coefficients (An > 0) are zero, reducing to a 0th order polynomial, or linear. To match the degraded stress-strain compression curve, a higher order polynomial is needed. Six conditions on stress were used (stress and its derivative at beginning, middle, and end of the curve) to obtain a 5th order polynomial, and then the derivative of that equation was taken to obtain modulus as a function of strain, yielding a 4th order polynomial that represents the degraded coating modulus vs. strain curve. For values of strain which exceed the failure strain observed in the laminate compression tests, the higher order polynomial will no longer match the test data. Therefore, after a specified effective-strain, representing failure, the modulus is defined to be the tangent of the polynomial curve. As a result, the stress/strain response has a continuous derivative, which aids in avoiding numerical instabilities. The test data does not clearly define the failure strain of the coating, but in the impact test it appears that the coating has a higher compressive failure strain in bending than the laminate failure strain. The two dominant modes of loading which cause coating loss on the impact side of the RCC (the front-side) are in-plane compression and transverse shear. The in-plane compression is measured by the peak out of plane tensile strain, ε3. As there is no direct loading of a shell element in this direction, ε3 is computed through Poisson’s relation 1−𝑣 (𝜀1 + 𝜀2) . When ε3 is tensile, it implies that the average of ε1 and ε2 is 𝜀3 = −𝑣 compressive. This failure mode will likely dominate when the RCC undergoes large bending, putting the front-side coating in high compressive strains. It is expected that a transverse shear failure mode will dominate when the debris source is very hard or very fast. By definition, the shell element cannot give a precise account of the transverse shear throughout the RCC’s thickness. However, the Belytschko-Tsay shell element formulation in LS-DYNA has a first-order approximation of transverse shear that is based on the out-of-plane nodal displacements and rotations that should suffice to give a qualitative evaluation of the transverse shear. By this formulation, the transverse shear is constant through the entire shell thickness and thus violates surface- traction conditions. The constitutive model implementation records the peak value of the tensile out-of-plane strain (ε3) and peak root-mean-sum transverse-shear: √𝜀13 2 . 2 + 𝜀23 *MAT_237 This is Material Type 237. This is a perfectly-matched layer (PML) material with a Biot linear hysteretic constitutive law, to be used in a wave-absorbing layer adjacent to a Biot hysteretic material (*MAT_BIOT_HYSTERETIC) in order to simulate wave propagation in an unbounded medium with material damping. This material is the visco-elastic counterpart of the elastic PML material (*MAT_PML_ELASTIC). See the Remarks *MAT_BIOT_HYSTERETIC sections of (*MAT_232) for further details. *MAT_PML_ELASTIC (*MAT_230) and Card 1 Variable MID 2 RO Type A8 F 3 E F 4 PR F 5 ZT F 6 FD F 7 8 Default none none none none 0.0 3.25 VARIABLE MID DESCRIPTION Material identification. A unique number or label not exceeding 8 characters must be specified. RO E PR ZT FD Mass density. Young’s modulus. Poisson’s ratio. Damping ratio Dominant excitation frequency in Hz *MAT_PERT_PIECEWISE_LINEAR_PLASTICITY This is Material Type 238. It is a duplicate of Material Type 24 (*MAT_PIECEWISE_- LINEAR_PLASTICITY) modified for use with *PERTURBATION_MATERIAL and solid elements in an explicit analysis. It should give exactly the same values as the original material, if used exactly the same. It exists as a separate material type because of the speed penalty (an approximately 10% increase in the overall execution time) associated with the use of a material perturbation. See Material Type 24 (*MAT_PIECEWISE_LINEAR_PLASTICITY) for a description of the material parameters. All of the documentation for Material Type 24 applies. Recommend practice is to first create the input deck using Material Type 24. Additionally, the CMP variable in the *PERTURBATION_MATERIAL must be set to affect a specific variables in the MAT_238 definition as defined in the following table; for example, CMP = 5 will perturb the yield stress. CMP value Material variable 3 5 6 7 E SIGY ETAN FAIL *MAT_COHESIVE_MIXED_MODE_ELASTOPLASTIC_RATE This is Material Type 240. This model is a rate-dependent, elastic-ideally plastic cohesive zone model. It includes a tri-linear traction-separation law with a quadratic yield and damage initiation criterion in mixed-mode loading, while the damage evolution is governed by a power-law formulation. It can be used only with cohesive element fomulations; see the variable ELFORM in *SECTION_SOLID and *SECTION_ SHELL. Card 1 1 2 3 4 5 6 7 8 Variable MID RO ROFLG INTFAIL EMOD GMOD THICK Type A8 Card 2 1 F 2 F 3 Variable G1C_0 G1C_INF EDOT_G1 Type F Card 3 1 F 2 F 3 F F 4 T0 F 4 5 T1 F 5 F 6 F 7 8 EDOT_T FG1 LCG1C F 6 F 7 F 8 Variable G2C_0 G2C_INF EDOT_G2 S0 S1 EDOT_S FG2 LCG2C Type F F F F F F F F VARIABLE MID DESCRIPTION Material identification. A unique number or label not exceeding 8 characters must be specified. RO Mass density ROFLG Flag for whether density is specified per unit area or volume. ROFLG = 0 specified density per unit volume (default), and ROFLG = 1 specifies the density is per unit area for controlling the mass of cohesive elements with an initial volume of zero. INTFAIL *MAT_COHESIVE_MIXED_MODE_ELASTOPLASTIC_RATE DESCRIPTION The number of integration points required for the cohesive element to be deleted. If it is zero, the element will not be deleted even if it satisfies the failure criterion. The value of INTFAIL may range from 1 to 4, with 1 the recommended value. EMOD The Young’s modulus of the material GMOD The shear modulus of the material THICK GT.0.0: Cohesive thickness LE.0.0: Initial thickness is calculated from nodal coordinates G1C_0 GT.0.0: Energy release rate GIC in Mode I LE.0.0: Lower bound value of rate-dependent GIC G1C_INF EDOT_G1 T0 T1 Upper bound value of rate-dependent 𝐺𝐼𝐶 (only considered if G1C_0 < 0) Equivalent strain rate at yield initiation to describe the rate dependency of GIC (only considered if G1C_0 < 0) GT.0.0: Yield stress in Mode I LT.0.0: Rate-dependency is considered, Parameter T0 Parameter T1, only considered if T0 < 0: GT.0.0: Quadratic logarithmic model LT.0.0: Linear logarithmic model EDOT_T Equivalent strain rate at yield initiation to describe the rate dependency of the yield stress in Mode I (only considered if T0 < 0) FG1 Parameter fG1 to describe the tri-linear shape of the traction- separation law in Mode I, see remarks. GT.0.0: FG1 is ratio of fracture energies 𝐺𝐼,𝑃/𝐺𝐼𝐶 LT.0.0: |FG1| is ratio of displacements (𝛿𝑛2 − 𝛿𝑛1)/(𝛿𝑛𝑓 − 𝛿𝑛1) LCG1C Load curve ID which defines fracture energy GIC as a function of cohesive element thickness. G1C_0 and G1C_INF are ignored in that case. Stress T, S En, Et Unloading Path Gp Gc n1, δ t1 n2, δ t2 nf, δ tf n, Δ Figure M240-1. Trilinear traction separation law DESCRIPTION GT.0.0: Energy release rate GIIC in Mode II LE.0.0: Lower bound value of rate-dependent GIIC VARIABLE G2C_0 G2C_INF Upper bound value of 𝐺𝐼𝐼𝐶 (only considered if G2C_0 < 0) EDOT_G2 Equivalent strain rate at yield initiation to describe the rate dependency of GIIC (only considered if G2C_0 < 0) S0 S1 GT.0.0: Yield stress in Mode II LT.0.0: Rate-dependency is considered, Parameter S0 Parameter S1, only considered if S0 < 0: GT.0.0: Quadratic logarithmic model is applied LT.0.0: Linear logarithmic model is applied EDOT_S Equivalent strain rate at yield initiation to describe the rate dependency of the yield stress in Mode II (only considered if S0 < 0) FG2 Parameter fG2 to describe the tri-linear shape of the traction- separation law in Mode II, see remarks. GT.0.0: FG2 is ratio of fracture energies 𝐺𝐼𝐼,𝑃/𝐺𝐼𝐼𝐶 LT.0.0: |FG2| is ratio of displacements (𝛿𝑡2 − 𝛿𝑡1)/(𝛿𝑡𝑓 − 𝛿𝑡1) Load curve ID which defines fracture energy GIIC as a function of cohesive element thickness. G2C_0 and G2C_INF are ignored in that case. *MAT_240 VARIABLE LCG2C Remarks: The model is a tri-linear elastic-ideally plastic Cohesive Zone Model, which was developed by Marzi et al. [2009]. It looks similar to *MAT_185, but considers effects of plasticity and rate-dependency. Since the entire separation at failure is plastic, no brittle fracture behavior can be modeled with this material type. The separations Δ𝑛 in normal (peel) and Δ𝑡 in tangential (shear) direction are calculated from the element’s separations in the integration points, and Δ𝑛 = max (un, 0) Δ𝑡 = √𝑢𝑡1 2 , 2 + 𝑢𝑡2 𝑢𝑛, 𝑢𝑡1 and 𝑢𝑡2 are the separations in normal and in the both tangential directions of the element coordinate system. The total (mixed-mode) separation Δ𝑚 is determined by Δ𝑚 = √Δ𝑛 2 + Δ𝑡 2. The initial stiffnesses in both modes are calculated from the elastic Young’s and shear moduli and are respectively, 𝐸𝑛 = 𝐸𝑡 = EMOD THICK GMOD THICK , where THICK, the element’s thickness, is an input parameter. Unless the input THICK > 0 it is calculated from the distance between the initial positions of the element’s corner nodes (Nodes 1-5, 2-6, 3-7 and 4-8, respectively). While the total energy under the traction-separation law is given by 𝐺𝐶, one further parameter is needed to describe the exact shape of the tri-linear material model. If the area (energy) under the constant stress (plateau) region is denoted 𝐺𝑃 , a parameter 𝑓𝐺 defines the shape of the traction-separation law, for mode I loading: 0 ≤ 𝑓𝐺1 = 𝐺𝐼,𝑃 𝐺𝐼𝐶 < 1 − 𝑇2 2𝐺𝐼𝐶𝐸𝑛 < 1 for mode II loading: 0 ≤ 𝑓𝐺2 = 𝐺𝐼𝐼,𝑃 𝐺𝐼𝐼𝐶 < 1 − 𝑆2 2𝐺𝐼𝐼𝐶𝐸𝑡 < 1 As a recommended alternative, the shape of the tri-linear model can be described by the following displacement ratios (triggered by negative input values for 𝑓𝐺): for mode I loading: 𝛿𝑛2 − 𝛿𝑛1 𝛿𝑛𝑓 − 𝛿𝑛1 0 < ∣𝑓𝐺1∣ = ∣ ∣ < 1 for mode II loading: 𝛿𝑡2 − 𝛿𝑡1 𝛿𝑡𝑓 − 𝛿𝑡1 0 < ∣𝑓𝐺2∣ = ∣ ∣ < 1 While 𝑓𝐺1 and 𝑓𝐺2 are always constant values, 𝑇, 𝑆, 𝐺𝐼𝐶 and 𝐺𝐼𝐼𝐶 may be chosen as functions of an equivalent strain rate 𝜀̇𝑒𝑞, which is evaluated by 𝜀̇𝑒𝑞 = √𝑢̇𝑛 2 + 𝑢̇𝑡2 2 + 𝑢̇𝑡1 THICK , where 𝑢̇𝑛, 𝑢̇𝑡1 and 𝑢̇𝑡2 are the velocities corresponding to the separations 𝑢𝑛, 𝑢𝑡1 and 𝑢𝑡2. For the yield stresses, two rate dependent formulations are implemented: 1. A quadratic logarithmic function: for mode I if T0 < 0 and T1 > 0: 𝑇(𝜀̇eq) = |T0| + |T1| [max (0, ln 𝜀̇eq EDOT_ T )] for mode II if S0 < 0 and S1 > 0: 𝑆(𝜀̇eq) = |S0| + |S1| [max (0, ln 𝜀̇eq EDOT_ S )] 2. A linear logarithmic function: for mode I if T0 < 0 and T1 < 0: 𝑇(𝜀̇eq) = |T0| + |T1|max (0, ln 𝜀̇eq EDOT_ T ) for mode II if S0 < 0 and S1 < 0: 𝜀̇eq EDOT_ S 𝑆(𝜀̇eq) = |S0| + |S1|max (0, ln ) Alternatively, T and S can be set to constant values: for mode I if T0 > 0: 𝑇(𝜀̇eq) = T0 for mode II if S0 > 0: 𝑆(𝜀̇eq) = SO The rate-dependency of the fracture energies are given by if G1C_ 0 < 0: 𝐺𝐼𝐶(𝜀̇eq) = |G1C_ 0| + (G1C_ INF − |G1C_ 0|)exp (− EDOT_ G1 𝜀̇eq ) if G2C_ 0 < 0: 𝐺𝐼𝐼𝐶(𝜀̇eq) = |G2C_ 0| + (G2C_ INF − |G2C_ 0|)exp (− EDOT_ G2 𝜀̇eq ) If positive values are chosen for G1C_0 or G2C_0, no rate-dependency is considered for this parameter and its value remains constant as specified by the user. As an alternative, fracture energies GIC and GIIC can be defined as functions of cohesive element thickness by using load curves LCG1C and LCG2C. In that case, parameters G1C_0, G1C_INF, G2C_0, and G2C_INF will be ignored and no rate dependence is considered. It should be noticed, that the equivalent strain rate 𝜀̇eq is updated until Δ𝑚 > 𝛿𝑚1, then the model behavior depends on the equivalent strain rate at yield initiation. Having defined the parameters describing the single modes, the mixed-mode behavior is formulated by quadratic initiation criteria for both yield stress and damage initiation, while the damage evolution follows a Power-Law. Traction n1 n2 nf Δn t1 m1 tf t2 Δt m2 mf Δm Figure M240-2. Trilinear mixed mode traction-separation law Due to reasons of readability, the following simplifications are made, 𝑇 = 𝑇(𝜀̇eq), 𝑆 = 𝑆(𝜀̇eq), 𝐺𝐼𝐶 = 𝐺𝐼𝐶(𝜀̇eq) and 𝐺𝐼𝐼𝐶 = 𝐺𝐼𝐼𝐶(𝜀̇eq). The mixed-mode yield initiation displacement 𝛿𝑚1 is defined as 𝛿𝑚1 = 𝛿𝑛1𝛿𝑡1√ 1 + 𝛽2 2 + (𝛽𝛿𝑛1)2 𝛿𝑡1 , are the single-mode yield initiation displacements and is the mixed-mode ratio. Analog to the yield initiation, the damage initiation and 𝛿𝑡1 = 𝑆 𝐸𝑡 where 𝛿𝑛1 = 𝑇 𝐸𝑛 𝛽 = displacement 𝛿𝑚2 is defined: Δ𝑡 Δ𝑛 𝛿𝑚2 = 𝛿𝑛2𝛿𝑡2√ 1 + 𝛽2 2 + (𝛽𝛿𝑛2)2 , 𝛿𝑡2 where 𝛿𝑛2 = 𝛿𝑛1 + 𝛿𝑡2 = 𝛿𝑡1 + 𝑓𝐺1𝐺𝐼𝐶 𝑓𝐺2𝐺𝐼𝐼𝐶 . With 𝛾 = arccos( ⟨𝑢𝑛⟩ Δ𝑚 ), the ultimate (failure) displacement 𝛿𝑚𝑓 can be written, 𝛿𝑚𝑓 = 𝛿𝑚1(𝛿𝑚1 − 𝛿𝑚2)𝐸𝑛𝐺𝐼𝐼𝐶cos2𝛾 + 𝐺𝐼𝐶(2𝐺𝐼𝐼𝐶 + 𝛿𝑚1(𝛿𝑚1 − 𝛿𝑚2)𝐸𝑡sin2𝛾) 𝛿𝑚1(𝐸𝑛𝐺𝐼𝐼𝐶cos2𝛾 + 𝐸𝑡𝐺𝐼𝐶sin2𝛾) . This formulation describes a power-law damage evolution with an exponent 𝜂 = 1.0 . After the shape of the mixed-mode traction-separation law has been determined by 𝛿𝑚1, 𝛿𝑚2 and 𝛿𝑚𝑓 , the plastic separation in each element direction, 𝑢𝑛,𝑃, 𝑢𝑡1,𝑃 and 𝑢𝑡2,𝑃 can be calculated. The plastic separation in peel direction is given by 𝑢𝑛,𝑃 = max(𝑢𝑛,𝑃,Δ𝑡−1, 𝑢𝑛 − 𝛿𝑚1cos (𝛾), 0). In shear direction, a shear yield separation 𝛿𝑡,𝑦, 𝛿𝑡,𝑦 = √(𝑢𝑡1 − 𝑢𝑡1,𝑃,Δ𝑡−1)2 + (𝑢𝑡2 − 𝑢𝑡2,𝑃,Δ𝑡−1)2, is defined. If 𝛿𝑡,𝑦 > 𝛿𝑚1sin𝛾, the plastic shear separations in the element coordinate system are updated, 𝑢𝑡1,𝑃 = 𝑢𝑡1,𝑃,Δ𝑡−1 + 𝑢𝑡1 − 𝑢𝑡1,Δ𝑡−1 𝑢𝑡2,𝑃 = 𝑢𝑡2,𝑃,Δ𝑡−1 + 𝑢𝑡2 − 𝑢𝑡2,Δ𝑡−1. In the formulas above, Δ𝑡 − 1 indicates the individual value from the last time increment. In case Δ𝑚 > 𝛿𝑚2, the damage initiation criterion is satisfied and a damage variable D increases monotonically, 𝐷 = max ( Δ𝑚 − 𝛿𝑚2 𝛿𝑚𝑓 − 𝛿𝑚2 , 𝐷Δ𝑡−1, 0). When Δ𝑚 > 𝛿𝑚𝑓 , complete damage (𝐷 = 1) is reached and the element fails in the corresponding integration point. Finally, the peel and the shear stresses in element directions are calculated, 𝜎𝑡1 = 𝐸𝑡(1 − 𝐷)(𝑢𝑡1 − 𝑢𝑡1,𝑃) 𝜎𝑡2 = 𝐸𝑡(1 − 𝐷)(𝑢𝑡2 − 𝑢𝑡2𝑃). In peel direction, no damage under pressure loads is considered if 𝑢𝑛 − 𝑢𝑛,𝑃 > 0 otherwise, Reference: 𝜎𝑛 = 𝐸𝑛(𝑢𝑛 − 𝑢𝑛,𝑃) 𝜎𝑛 = 𝐸𝑛(1 − 𝐷)(𝑢𝑛 − 𝑢𝑛,𝑃) S. Marzi, O. Hesebeck, M. Brede and F. Kleiner (2009), A Rate-Dependent, Elasto- Plastic Cohesive Zone Mixed-Mode Model for Crash Analysis of Adhesively Bonded Joints, In Proceeding: 7th European LS-DYNA Conference, Salzburg *MAT_JOHNSON_HOLMQUIST_JH1 This is Material Type 241. This Johnson-Holmquist Plasticity Damage Model is useful for modeling ceramics, glass and other brittle materials. This version corresponds to the original version of the model, JH1, and Material Type 110 corresponds to JH2, the updated model. Card 1 1 Variable MID Type A8 Card 2 1 Variable EPSI Type F Card 3 1 2 RO F 2 T F 2 Variable EPFMIN EPFMAX Type F F VARIABLE MID 8 C F 8 8 3 G F 3 4 P1 F 4 5 S1 F 5 6 P2 F 6 7 S2 F 7 ALPHA SFMAX BETA DP1 F 7 F F F F 3 K1 F 4 K2 F 5 K3 F 6 FS F DESCRIPTION Material identification. A unique number or label not exceeding 8 characters must be specified. RO Density. G P1 S1 P2 S2 Shear modulus. Pressure point 1 for intact material. Effective stress at P1. Pressure point 2 for intact material. Effective stress at P2. Intact material strength (D < 0) (P1, S1) (P2, S2) (P3, S3) . ε*>1 . ε*=1 . ε*>1 . ε*=1 Fractured material strength (D ≥ 0) ALPHA (T, 0) Pressure Figure M241-1. Strength: equivalent stress versus pressure. VARIABLE DESCRIPTION C EPSI T Strain rate sensitivity factor. Quasi-static threshold strain rate. See *MAT_015. Maximum tensile pressure strength. This value is positive in tension. ALPHA Initial slope of the fractured material strength curve. See Figure M241-1. SFMAX Maximum strength of the fractured material. BETA DP1 Fraction of elastic energy loss converted to hydrostatic energy (affects bulking pressure (history variable 1) that accompanies damage). Maximum compressive pressure strength. This value is positive in compression. EPFMIN Plastic strain for fracture at tensile pressure 𝑇. See Figure M241-2. EPFMAX Plastic strain for fracture at compressive pressure DP1. See Figure M241-1. K1 K2 First pressure coefficient (equivalent to the bulk modulus). Second pressure coefficient. ) fp ( (DP1, EPFMAX) (T, EPFMIN) Pressure Figure M241-2. Fracture strain versus pressure. VARIABLE DESCRIPTION K3 FS Third pressure coefficient. Element deletion criteria. LT.0: delete if P < FS (tensile failure). EQ.0: no element deletion (default). GT.0: delete element if the 𝜀̅𝑝> FS. Remarks: The equivalent stress for both intact and fractured ceramic-type materials is given by 𝜎𝑦 = (1 + 𝑐 ln 𝜀̇∗)𝜎(𝑃) where 𝜎(𝑃) is evaluated according to Figure M241-1. 𝑝 (𝑃) 𝐷 = ∑ Δ𝜀𝑝/𝜀𝑓 represents the accumulated damage (history variable 2) based upon the increase in plastic strain per computational cycle and the plastic strain to fracture is evaluated according to Figure M241-2. In undamaged material, the hydrostatic pressure is given by in compression and by 𝑃 = 𝑘1𝜇 + 𝑘2𝜇2 + 𝑘3𝜇3 + 𝛥𝑃 𝑃 = 𝑘1𝜇 + 𝛥𝑃 in tension where 𝜇 = 𝜌 𝜌0 − 1 . A fraction, between 0 and 1, of the elastic energy loss, 𝛽, is converted into hydrostatic potentiall energy (pressure). The pressure increment, 𝛥𝑃, associated with the increment in the hydrostatic potential energy is calculated at ⁄ 𝑓 are the intact and failed yield stresses respectively. This fracture, where 𝜎𝑦 and 𝜎𝑦 pressure increment is applied both in compression and tension, which is not true for JH2 where the increment is added only in compression. 𝛥𝑃 = −𝑘1𝜇𝑓 + √(𝑘1𝜇𝑓 ) + 2𝛽𝑘1𝛥𝑈 𝛥𝑈 = 𝜎𝑦 − 𝜎𝑦 6𝐺 *MAT_KINEMATIC_HARDENING_BARLAT2000 This is Material Type 242. This model combines Yoshida non-linear kinematic hardening rule (*MAT_125) with the 8-parameter material model of Barlat and Lian (2003) (*MAT_133) to model metal sheets under cyclic plasticity loading and with anisotropy in plane stress condition. Also see manual pages in *MAT_226. Card 1 1 Variable MID Type I 2 RO F 3 E F 4 PR F 5 6 8 7 M F Default none 0.0 0.0 0.0 none Card 2 1 2 3 4 5 6 7 8 Variable ALPHA1 ALPHA2 ALPHA3 ALPHA4 ALPHA5 ALPHA6 ALPHA7 ALPHA8 Type F F F F F F F I Default 0.0 0.0 0.0 0.0 0.0 0.0 0.0 none Card 3 1 2 3 4 5 6 7 8 Variable Type Default Card 4 1 2 3 4 5 6 7 8 Variable Type Default Card 5 Variable 1 CB Type F 2 Y F 3 C F 4 K F 5 RSAT F 6 SB F 7 H F 8 Default none none none none none none none Card 6 1 2 3 Variable AOPT Type I IOPT I 4 C1 F 5 C2 F Default none none 0.0 0.0 6 7 8 Card 7 Variable 1 XP Type F 2 YP F 3 ZP F 4 A1 F 5 A2 F 6 A3 F 7 8 Default none none none none none none Card 8 Variable 1 V1 Type F 2 V2 F 3 V3 F 4 D1 F 5 D2 F 6 D3 F 7 8 Default none none none none none none VARIABLE DESCRIPTION MID RO E PR M ALPHA1 ALPHA2 ALPHA3 ALPHA4 ALPHA5 ALPHA6 ALPHA7 ALPHA8 CB Y SC K RSAT SB Material identification. A unique number must be specified. Mass density. Young’s modulus, E. Poisson’s ratio, ν. Flow potential exponent. For face centered cubic (FCC) materials m = 8 is recommended and for body centered cubic (BCC) materials m = 6 may be used. α1, material constant in Barlat’s yield equation. α2, material constant in Barlat’s yield equation. α3, material constant in Barlat’s yield equation. α4, material constant in Barlat’s yield equation. α5, material constant in Barlat’s yield equation. α6, material constant in Barlat’s yield equation. α7, material constant in Barlat’s yield equation. α8, material constant in Barlat’s yield equation. The uppercase B defined in the Yoshida’s equations. Anisotropic parameter stagnation, defined in the Yoshida’s equations. associated with work-hardening The lowercase c defined in the Yoshida’s equations. Hardening parameter as defined in the Yoshida’s equations. Hardening parameter as defined in the Yoshida’s equations. The lowercase b as defined in the Yoshida’s equations. H AOPT *MAT_KINEMATIC_HARDENING_BARLAT2000 DESCRIPTION Anisotropic parameter stagnation, defined in the following Yoshida’s equations. associated with work-hardening Material axes option : EQ.0.0: locally orthotropic with material axes determined by element nodes 1, 2, and 4, as with *DEFINE_COORDI- NATE_NODES. EQ.2.0: globally orthotropic with material axes determined by vectors defined below, as with *DEFINE_COORDI- NATE_VECTOR. EQ.3.0: locally orthotropic material axes determined by rotating the material axes about the element normal by an angle, BETA, from a line in the plane of the element defined by the cross product of the vector v with the element normal. LT.0.0: the absolute value of AOPT is a coordinate system ID number (CID on *DEFINE_COORDINATE_NODES, *DEFINE_COORDINATE_SYSTEM or *DEFINE_CO- ORDINATE_VECTOR). Available with the R3 release of Version 971 and later. IOPT Kinematic hardening rule flag: EQ.0: Original Yoshida formulation. EQ.1: Modified formulation. Define C1, C2 below. C1, C2 Constants used to modify R: 𝑅 = RSAT × [(𝐶1 + 𝜀̅𝑝)𝑐2 − 𝐶1 𝑐2] Coordinates of point p for AOPT = 1. Components of vector a for AOPT = 2. Components of vector v for AOPT = 3. Components of vector d for AOPT = 2. XP, YP, ZP A1, A2, A3 V1, V2, V3 D1, D2, D3 Remarks: 1. A total of eight parameters (α1 to α8) are needed to describe the yield surface. The parameters can be determined with tensile tests in three directions and an equal biaxial tension test. For detailed theoretical background and material parameters of some typical FCC materials, please see remarks in *MAT_133 and Barlat’s 2003 paper. 2. NUMISHEET 2005 provided a complete set of the parameters of AL5182-O for Benchmark #2, the cross member, as below (flow potential exponent M = 8): α1 0.94 α2 1.08 α3 0.97 α4 1.0 α5 1.0 α6 1.02 α7 1.03 α8 1.11 3. For a more detailed description on the Yoshida model and parameters, please see Remarks in *MAT_226 and *MAT_125. 4. For information on variable AOPT please see remarks in *MAT_226. 5. To improve convergence, it is recommended that *CONTROL_IMPLICIT_- FORMING type ‘1’ be used when conducting springback simulation. 6. This material model is available in LS-DYNA R5 Revision 58432 or later releases. *MAT_HILL_90 This is Material Type 243. This model was developed by Hill [1990] for modeling sheets with anisotropic materials under plane stress conditions. This material allows the use of the Lankford parameters for the definition of the anisotropy. All features of this model are the same as in *MAT_036, only the yield condition and associated flow rules are replaced by the Hill90 equations. Card 1 1 Variable MID Type A8 Card 2 Variable Type 1 M F 2 RO F 2 3 E F 3 4 PR F 4 5 HR F 5 R00 / AH R45 / BH R90 / CH LCID F F F I 6 P1 F 6 E0 F 7 P2 F 7 SPI F 8 ITER F 8 P3 F Hardening Card. Additional Card for M < 0. Card 3 1 2 3 4 5 6 7 8 Variable CRC1 CRA1 CRC2 CRA2 CRC3 CRA3 CRC4 CRA4 Type F Card 4 1 Variable AOPT Type F F 2 C F F 5 F 3 P F F 4 VLCID I F 6 FLAG F F 7 F 1 2 3 Variable Type Card 6 Variable 1 V1 Type F 2 V2 F 3 V3 F This card is optional. 4 A1 F 4 D1 F 5 A2 F 5 D2 F 6 A3 F 6 D3 F *MAT_243 7 8 7 8 BETA F Card 6 1 2 3 4 5 6 7 8 Variable USRFAIL Type F VARIABLE DESCRIPTION MID RO E Material identification. A unique number or label not exceeding 8 characters must be specified. Mass density. Young’s modulus, E GT.0.0: Constant value, LT.0.0: Load curve ID = (-E) which defines Young’s Modulus as a function of plastic strain. See Remark 1. PR Poisson’s ratio, ν *MAT_HILL_90 DESCRIPTION HR Hardening rule: EQ.1.0: linear (default), EQ.2.0: exponential (Swift) EQ.3.0: load curve or table with strain rate effects EQ.4.0: exponential (Voce) EQ.5.0: exponential (Gosh) EQ.6.0: exponential (Hocket-Sherby) EQ.7.0: load curves in three directions EQ.8.0: table with temperature dependence EQ.9.0: 3d table with temperature and strain rate dependence P1 Material parameter: HR.EQ.1.0: Tangent modulus, HR.EQ.2.0: k, strength coefficient hardening for Swift exponential HR.EQ.4.0: a, coefficient for Voce exponential hardening HR.EQ.5.0: k, strength coefficient hardening for Gosh exponential HR.EQ.6.0: a, coefficient for Hocket-Sherby exponential hardening HR.EQ.7.0: load curve ID for hardening in 45 degree direction. See Remark 2. P2 Material parameter: HR.EQ.1.0: Yield stress HR.EQ.2.0: n, exponent for Swift exponential hardening HR.EQ.4.0: c, coefficient for Voce exponential hardening HR.EQ.5.0: n, exponent for Gosh exponential hardening HR.EQ.6.0: c, coefficient for Hocket-Sherby exponential hardening HR.EQ.7.0: load curve ID for hardening in 90 degree direction. See Remark 2. DESCRIPTION ITER Iteration flag for speed: ITER.EQ.0.0: fully iterative ITER.EQ.1.0: fixed at three iterations *MAT_243 M CRCn CRAn R00 Generally, ITER = 0 is recommended. However, ITER = 1 is somewhat faster and may give acceptable results in most problems. m, exponent in Hill’s yield surface, absolute value is used if negative. Typically, m ranges between 1 and 2 for low-r materials, such as aluminum (AA6111: m≈1.5), and is greater than 2 for high r-values, as in steel (DP600: m≈4). Chaboche-Rousselier hardening parameters, see remarks. Chaboche-Rousselier hardening parameters, see remarks. R00, Lankford parameter in 0 degree direction GT.0.0: Constant value, LT.0.0: Load curve or Table ID = (-R00) which defines R value as a function of plastic strain (Curve) or as a function of temperature and plastic strain (Table). See Remark 3. R45 R45, Lankford parameter in 45 degree direction GT.0.0: Constant value, LT.0.0: Load curve or Table ID = (-R45) which defines R value as a function of plastic strain (Curve) or as a function of temperature and plastic strain (Table). See Remarks 2 and 3. R90 R90, Lankford parameter in 90 degree direction GT.0.0: Constant value, LT.0.0: Load curve or Table ID = (-R90) which defines R value as a function of plastic strain (Curve) or as a function of temperature and plastic strain (Table). See Remarks 2 and 3. AH BH a, Hill90 parameter, which is read instead of R00 if FLAG = 1. b, Hill90 parameter, which is read instead of R45 if FLAG = 1. CH LCID *MAT_HILL_90 DESCRIPTION c, Hill90 parameter, which is read instead of R90 if FLAG = 1. Load curve/table ID for hardening in the 0 degree direction. See Remark 1. E0 Material parameter HR.EQ.2.0: 𝜀0 for determining initial yield stress for Swift exponential hardening. (Default = 0.0) HR.EQ.4.0: b, coefficient for Voce exponential hardening HR.EQ.5.0: 𝜀0 for determining initial yield stress for Gosh exponential hardening. (Default = 0.0) HR.EQ.6.0: b, coefficient for Hocket-Sherby exponential hardening SPI if 𝜀0 is zero above and HR = 2.0. (Default = 0.0) ⁄ (𝑛−1) EQ.0.0: 𝜀0 = ⎜⎜⎜⎛𝐸 𝑘⁄ ⎝ ⎟⎟⎟⎞ ⎠ LE.0.02: 𝜀0 = SPI GT.0.02: 𝜀0 = 1 𝑛⁄ ⎜⎜⎜⎛SPI ⁄ ⎝ ⎟⎟⎟⎞ ⎠ If HR = 5.0 the strain at plastic yield is determined by an iterative procedure based on the same principles as for HR.EQ.2.0. P3 Material parameter: HR.EQ.5.0: p, parameter for Gosh exponential hardening HR.EQ.6.0: n, exponent for Hocket-Sherby exponential hardening AOPT Material axes option : EQ.0.0: locally orthotropic with material axes determined by element nodes 1, 2, and 4, as with *DEFINE_COORDI- NATE_NODES, and then rotated about the shell ele- ment normal by the angle BETA. EQ.2.0: globally orthotropic with material axes determined by vectors defined below, as with *DEFINE_COORDI- C P VLCID FLAG *MAT_243 DESCRIPTION NATE_VECTOR. EQ.3.0: locally orthotropic material axes determined by rotating the material axes about the element normal by an angle, BETA, from a line in the plane of the element defined by the cross product of the vector v with the element normal. LT.0.0: the absolute value of AOPT is a coordinate system ID number (CID on *DEFINE_COORDINATE_NODES, *DEFINE_COORDINATE_SYSTEM or *DEFINE_CO- ORDINATE_VECTOR). Available with the R3 release of Version 971 and later. C in Cowper-Symonds strain rate model p in Cowper-Symonds strain rate model, p = 0.0 for no strain rate effects Volume correction curve ID defining the relative volume change (change in volume relative to the initial volume) as a function of the effective plastic strain. This is only used when nonzero. See Remark 1. Flag for interpretation of parameters. If FLAG = 1, parameters AH, BH, and CH are read instead of R00, R45, and R90. See Remark 4. XP, YP, ZP Coordinates of point p for AOPT = 1. A1, A2, A3 Components of vector a for AOPT = 2. V1, V2, V3 Components of vector v for AOPT = 3. D1, D2, D3 Components of vector d for AOPT = 2. BETA Material angle in degrees for AOPT = 0 and 3, may be overridden on the element card, see *ELEMENT_SHELL_BETA. USRFAIL User defined failure flag USRFAIL.EQ.0: no user subroutine is called USRFAIL.EQ.1: user subroutine matusr_24 in dyn21.f is called *MAT_HILL_90 1. The effective plastic strain used in this model is defined to be plastic work equivalent. A consequence of this is that for parameters defined as functions of effective plastic strain, the rolling (00) direction should be used as reference direction. For instance, the hardening curve for HR = 3 is the stress as function of strain for uniaxial tension in the rolling direction, VLCID curve should give the relative volume change as function of strain for uniaxial tension in the roll- ing direction and load curve given by -E should give the Young’s modulus as function of strain for uniaxial tension in the rolling direction. Optionally the curve can be substituted for a table defining hardening as function of plastic strain rate (HR = 3) or temperature (HR = 8). 2. Exceptions from the rule above are curves defined as functions of plastic strain in the 45 and 90 directions, i.e., P1 and P2 for HR = 7 and negative R45 or R90. The hardening curves are here defined as measured stress as function of meas- ured plastic strain for uniaxial tension in the direction of interest, i.e., as deter- mined from experimental testing using a standard procedure. Moreover, the curves defining the R values are as function of the measured plastic strain for uniaxial tension in the direction of interest. These curves are transformed in- ternally to be used with the effective stress and strain properties in the actual model. The effective plastic strain does not coincide with the plastic strain components in other directions than the rolling direction and may be somewhat confusing to the user. Therefore the von Mises work equivalent plastic strain is output as history variable #2 if HR = 7 or if any of the R-values is defined as function of the plastic strain. 3. The R-values in curves are defined as the ratio of instantaneous width change to instantaneous thickness change. That is, assume that the width W and thick- ness T are measured as function of strain. Then the corresponding R-value is given by: 𝑅 = 𝑑𝑊 𝑑𝜀 𝑑𝑇 𝑑𝜀 /𝑊 /𝑇 4. The anisotropic yield criterion Φ for plane stress is defined as: Φ = 𝐾1 𝑚 + 𝐾3𝐾2 (𝑚/2)−1 + 𝑐𝑚𝐾4 𝑚/2 = (1 + 𝑐𝑚 − 2𝑎 + 𝑏)𝜎𝑌 𝑚 where 𝜎𝑌 is the yield stress and Ki = 1,4 are given by: 𝐾1 = ∣𝜎𝑥 + 𝜎𝑦∣ 𝐾2 = ∣𝜎𝑥 2 + 𝜎𝑦 2 ∣ 2 + 2𝜎𝑥𝑦 𝐾3 = −2𝑎(𝜎𝑥 2 − 𝜎𝑦 2) + 𝑏(𝜎𝑥 − 𝜎𝑦) 𝐾4 = ∣(𝜎𝑥 − 𝜎𝑦) 2 ∣ + 4𝜎𝑥𝑦 If FLAG = 0, the anisotropic material constants a, b, and c are obtained through R00, R45, and R90 using these 3 equations: 1 + 2𝑅00 = 𝑐𝑚 − 𝑎 + {(𝑚 + 2)/2𝑚}𝑏 1 − 𝑎 + {(𝑚 − 2)/2𝑚}𝑏 1 + 2𝑅45 = 𝑐𝑚 1 + 2𝑅90 = 𝑐𝑚 + 𝑎 + {(𝑚 + 2)/2𝑚}𝑏 1 + 𝑎 + {(𝑚 − 2)/2𝑚}𝑏 If FLAG = 1, material parameters a (AH), b (BH), and c (CH) are used directly. For material parameters a, b, c, and m, the following condition has to be ful- filled, otherwise an error termination occurs: 1 + 𝑐𝑚 − 2𝑎 + 𝑏 > 0 Two even more strict conditions should ensure convexity of the yield surface according to Hill (1990). A warning message will be dumped if at least one of them is violated: 𝑏 > −2 (𝑚 )−1 𝑐𝑚 𝑏 > 𝑎2 − 𝑐𝑚 The yield strength of the material can be expressed in terms of k and n: 𝜎𝑌 = 𝑘𝜀𝑛 = 𝑘(𝜀𝑦𝑝 + 𝜀̅𝑝) where 𝜀𝑦𝑝 is the elastic strain to yield and 𝜀̅𝑝 is the effective plastic strain (loga- rithmic). If SIGY is set to zero, the strain to yield if found by solving for the intersection of the linearly elastic loading equation with the strain hardening equation: which gives the elastic strain at yield as: 𝜎 = 𝐸𝜀 𝜎 = 𝑘𝜀𝑛 𝜀𝑦𝑝 = ( [ 1 ] 𝑛−1 ) If SIGY yield is nonzero and greater than 0.02 then: 𝜀𝑦𝑝 = ( 𝜎𝑌 [1 𝑛] ) The other available hardening models include the Voce equation given by 𝜎Y(𝜀𝑝) = 𝑎 − 𝑏𝑒−𝑐𝜀𝑝, the Gosh equation given by 𝜎Y(𝜀𝑝) = 𝑘(𝜀0 + 𝜀𝑝)𝑛 − 𝑝, and finally the Hocket-Sherby equation given by 𝜎Y(𝜀𝑝) = 𝑎 − 𝑏𝑒−𝑐𝜀𝑝 . For the Gosh hardening law, the interpretation of the variable SPI is the same, i.e., if set to zero the strain at yield is determined implicitly from the intersec- tion of the strain hardening equation with the linear elastic equation. To include strain rate effects in the model we multiply the yield stress by a factor depending on the effective plastic strain rate. We use the Cowper- Symonds’ model, hence the yield stress can be written 𝜎Y(𝜀𝑝, 𝜀̇𝑝) = 𝜎Y ⎡1 + ( ⎢ ⎣ 𝑠 denotes the static yield stress, 𝐶 and 𝑝 are material parameters, 𝜀̇𝑝 is 𝑠 (𝜀𝑝) ⎤ ⎥ ⎦ ) 1/𝑝 𝜀̇𝑝 where 𝜎Y the effective plastic strain rate. 5. A kinematic hardening model is implemented following the works of Chaboche and Roussilier. A back stress α is introduced such that the effective stress is computed as 𝜎eff = 𝜎eff(𝜎11 − 2𝛼11 − 𝛼22, 𝜎22 − 2𝛼22 − 𝛼11, 𝜎12 − 𝛼12) The back stress is the sum of up to four terms according to 𝛼𝑖𝑗 = ∑ 𝛼𝑖𝑗 𝑘=1 and the evolution of each back stress component is as follows 𝛿𝛼𝑖𝑗 𝑘 = 𝐶𝑘 (𝑎𝑘 𝑠𝑖𝑗 𝜎eff − 𝛼𝑖𝑗 𝑘 ) 𝛿𝜀𝑝 where 𝐶𝑘 and 𝑎𝑘 are material parameters,𝑠𝑖𝑗 is the deviatoric stress tensor, 𝜎eff is the effective stress and 𝜀𝑝 is the effective plastic strain. *MAT_244 This material model is developed for both shell and solid models. It is mainly suited for hot stamping processes where phase transformations are crucial. It has five phases and it is assumed that the blank is fully austenitized before cooling. The basic constitutive model is based on the work done by P. Akerstrom [2, 7]. Automatic switching between cooling and heating of the blank is under development. To activate the heating algorithm, set HEAT = 1 or 2 and add the appropriate input Cards. See the description of the HEAT parameter below. HEAT = 0 as is the default activates only the cooling algorithm and no extra cards need to be read in. Also note that for HEAT = 0 you must check that the initial temperature of this material is above the start temperature for the ferrite transformation. The transformation temperatures are echoed in the messag and in the d3hsp file. If HEAT > 0 the temperature that instantaneous transform all ferrite back to austenite is also echoed in the messag file. If you want to heat up to 100% austenite you must let the specimen’s temperature exceed that temperature. Features Added in 2014: 1. Young’s modulus and Poisson ratio can now be given as temperature dependent load curves or by a table definition with a load curve for each phase. See Remark 8. 2. Latent heat can now be given for each phase. See Remark 9. 3. Thermal expansion can now be given for each phase Remark 10. 4. Advanced reaction kinetic modifications include the ability to tailor the start temperatures and the activation energies. The martensite start temperature can be dependent on the plastic strain and triaxiality, and the activation energies can be scaled with the plastic strain as well. 5. Hardness calculation improved when tempering is active. Improvements are achieved in the bainite and martensite phases (experimental). See Remark 11. NOTE: For this material “weight%” means “ppm × 10-4”. 1 Variable MID Type I 2 RO F 3 E F 4 PR F *MAT_UHS_STEEL 5 6 7 8 TUNIT CRSH PHASE HEAT Defaults none none none none 3600 Card 2 1 2 3 4 5 F I 0 6 I 0 7 Variable LCY1 LCY2 LCY3 LCY4 LCY5 KFER KPER Type I I I I I F F I 0 8 B F Defaults none none none none none 0.0 0.0 0.0 Card 3 Variable Type 1 C F 2 Co F 3 Mo F 4 Cr F 5 Ni F 6 Mn F 7 Si F 8 V F Defaults 0.0 0.0 0.0 0.0 0.0 0.0 0.0 0.0 Card 4 Variable Type 1 W F 2 Cu F 3 P F 4 Al F 5 As F 6 Ti F Defaults 0.0 0.0 0.0 0.0 0.0 0.0 7 8 CWM LCTRE I 0 I none Card 5 1 2 3 4 5 6 7 8 Variable THEXP1 THEXP5 LCTH1 LCTH5 TREF LAT1 LAT5 TABTH Type F F I I F F F I Defaults 0.0 0.0 none none 273.15 0.0 0.0 none Card 6 1 2 3 4 5 6 7 8 Variable QR2 QR3 QR4 ALPHA GRAIN TOFFE TOFPE TOFBA Type F F F F F F F F Defaults 0.0 0.0 0.0 0.0 0.0 0.0 0.0 0.0 Card 7 1 2 3 4 5 6 7 8 Variable PLMEM2 PLMEM3 PLMEM4 PLMEM5 STRC STRP REACT TEMPER Type I F F F F F Defaults 0.0 0.0 0.0 0.0 0.0 0.0 I 0 I 0 Heat Card 1. Additional Card for HEAT = 1. Card 8 1 2 3 4 5 6 7 8 Variable AUST FERR PEAR BAIN MART GRK GRQR TAU1 Type F F F F F F F F Default 0.0 0.0 0.0 0.0 0.0 0.0 0.0 2.08E+8 Heat Card 2. Additional Card for HEAT =1. Card 9 1 2 3 4 5 6 7 8 Variable GRA GRB EXPA EXPB GRCC GRCM HEATN TAU2 Type F F F F F F F F Default 3.11 7520. 1.0 1.0 none none 1.0 4.806 Reaction Card. Addition card for REACT = 1. Card 10 Variable 1 FS Type F 2 PS F 3 BS F 4 5 6 7 8 MS MSIG LCEPS23 LCEPS4 LCEPS5 F F I I I Default 0.0 0.0 0.0 0.0 none none none none Tempering Card. Additional card for TEMPR = 1. Card 11 1 2 3 4 5 6 7 8 Variable LCH4 LCH5 DTCRIT TSAMP Type Default I 0 I 0 F F 0.0 0.0 Computational Welding Mechanics Card. Additional card for CWM = 1. Card 11 1 2 3 4 5 6 7 8 Variable TASTART TAEND TLSTART TLEND EGHOST PGHOST AGHOST Type F F F F F F F Default 0.0 0.0 0.0 0.0 0.0 0.0 0.0 VARIABLE DESCRIPTION BASELINE VALUE MID RO E Material ID, a unique number has to be chosen. Material density Youngs’ modulus: GT.0.0: constant value is used LT.0.0: LCID or TABID. Temperature dependent Youngs’ modulus given by load curve ID = -E or a Table ID = -E. When using a table to describe the Youngs for modulus see Remark 8 more information. 7830 Kg/m3 100 GPa [1] PR Poisson’s ratio: 0.30 [1] GT.0.0: constant value LT.0.0: LCID or TABID: Temperature dependent Poisson ratio given by load curve or table ID = -PR. The table input is described in Remark 8. Number of time units per hour. Default is seconds, that is 3600 time units per It is used only for hardness hour. calculations. TUNIT 3600. CRSH *MAT_UHS_STEEL DESCRIPTION BASELINE VALUE Switch to use a simple and fast material model but with the actual phases active. EQ.0: The original model where phase transitions are active and trip is used. EQ.1: A simpler and faster version. This option is mainly when transferring the quenched blank into a crash analysis where all properties from the cooling are maintained. This option must be *INTERFACE_- used with a SPRINGBACK keyword and should be used after a quenching analysis. EQ.2: Same as 0 but trip effect is not used. 0 0 PHASE Switch to include or exclude middle phases from the simulation. EQ.0: All phases active (default) EQ.1: pearlite and bainite excluded EQ.2: bainite excluded EQ.3: ferrite and pearlite excluded EQ.4: ferrite and bainite excluded EQ.5: exclude middle phases (only austenite → martensite) VARIABLE DESCRIPTION BASELINE VALUE HEAT Switch to activate the heating algorithms EQ.0: Heating is not activated. That means that no transformation to Austenite is possible. EQ.1: Heating is activated: That means that only transformation to Austenite is possible. EQ.2: Automatic switching between cooling and heating. LS-DYNA checks the temperature gradient and calls the appropriate algo- rithms. For example, this can be used to simulate the heat affect- ed zone during welding. LT.0: Switch between cooling and heating is defined by a time de- pendent id The ordinate ABS(HEAT). should be 1.0 when heating is applied and 0.0 if cooling is pref- erable. load curve with LCY1 Load curve or Table ID for austenite hardening. [5] IF LCID input yield stress versus effective plastic strain. IF TABID.GT.0: 2D table. Input temperatures as table values and hardening curves as targets for those temperatures IF TABID.LT.0: 3D table. Input temperatures as main table values and strain rates as values for the sub tables, and hardening curves as targets for those strain rates. VARIABLE DESCRIPTION BASELINE VALUE LCY2 LCY3 LCY4 LCY5 KFERR KPEAR B C Co Mo Cr Ni Mn Si V W Cu P Al As Ti Load curve ID for ferrite hardening (stress versus eff. pl. str.) Load curve or Table ID for pearlite. See LCY1 for description. Load curve or Table ID for bainite. See LCY1 for description. Load curve or Table ID for martensite. See LCY1 for description. Correction factor for boron in the ferrite reaction. Correction factor for boron in the pearlite reaction. Boron [weight %] Carbon [weight %] Cobolt [weight %] Molybdenum [weight %] Chromium [weight %] Nickel [weight %] Manganese [weight %] Silicon [weight %] Vanadium [weight %] Tungsten [weight %] copper [weight %] Phosphorous [weight %] Aluminium [weight %] Arsenic [weight %] Titanium [weight %] 1.9 × 105 [2] 3.1 × 103 [2] 0.003 [2, 4] 0.23 [2, 4] 0.0 [2, 4] 0.0 [2, 4] 0.21 [2, 4] 0.0 [2, 4] 1.25 [2, 4] 0.29 [2, 4] 0.0 [2, 4] 0.0 0.0 0.013 0.0 0.0 0.0 VARIABLE CWM LCTRE THEXP1 THEXP5 LCTH1 LCTH5 TREF LAT1 DESCRIPTION BASELINE VALUE for Flag computational welding mechanics input. One additional input card is read. EQ.1.0: Active EQ.0.0: Inactive Load curve for transformation induced for more strains. information. See Remark 13 Coefficient of austenite Coefficient of martensite thermal expansion in 25.1 × 10−6 1/K [7] thermal expansion in 11.1 × 10−6 1/K [7] 0 0 293.15 590 × 106 J/m3 [2] the Load curve coefficient for austenite: for thermal expansion LT.0.0: curve ID = -LA and TREF is used as reference temperature GT.0.0: curve ID = LA Load curve coefficient for martensite: the for thermal expansion LT.0.0: curve ID = -LA and TREF is used as reference temperature GT.0.0: curve ID = LA temperature thermal Reference expansion. Used if and only if LA.LT.0.0 or/and LM.LT.0.0 for Latent heat for the decomposition of austenite into ferrite, pearlite and bainite. GT.0.0: Constant value LT.0.0: Curve ID or Table ID. See infor- for more Remark 9 mation. LAT5 TABTH QR2 QR3 QR4 ALPHA GRAIN TOFFE 2-1220 (EOS) DESCRIPTION Latent heat for the decomposition of austenite into martensite. GT.0.0: Constant value LT.0.0: Curve ID: Note that LAT 5 is ignored if a Table ID is used in LAT1. for thermal expansion Table definition coefficient. With this option active THEXP1, THEXP2, LCTH1 and LCTH5 are ignored. See Remark 10. GT.0: A table for instantaneous thermal expansion (TREF is ignored). LT.0: A table with thermal expansion with reference to TREF. energy divided by Activation the universal gas constant for the diffusion reaction of the austenite-ferrite reaction: Q2/R. R = 8.314472 [J/mol K]. energy divided by the Activation universal gas constant for the diffusion reaction austenite-pearlite the reaction: Q3/R. R = 8.314472 [J/mol K]. for energy divided by Activation the universal gas constant for the diffusion reaction for the austenite-bainite reaction: Q4/R. R = 8.314472 [J/mol K]. for Material constant the martensite phase. A value of 0.011 means that 90% of the available austenite is transformed into martensite at 210 degrees below the martensite start temperature , whereas a value of 0.033 means a 99.9% transformation. ASTM grain size number for austenite, usually a number between 7 and 11. Number of degrees that the ferrite is bleeding over into the pearlite reaction. *MAT_UHS_STEEL BASELINE VALUE 640 × 106 J/m3 [2] 10324 K [3] = (23000 cal/mole) × (4.184 J/cal) / (8.314 J/mole/K) 13432. K [3] 15068. K [3] 0.011 6.8 VARIABLE DESCRIPTION BASELINE VALUE TOFPE TOFBA PLMEM2 PLMEM3 PLMEM4 PLMEM5 Number of degrees that the pearlite is bleeding over into the bainite reaction Number of degrees that the bainite is bleeding over the martensite into reaction. Memory coefficient for the plastic strain that is carried over from the austenite. A value of 1 means that all plastic strains from austenite is transferred to the ferrite phase and a value of 0 means that nothing is transferred. Same as PLMEM2 but between austenite and pearlite. Same as PLMEM2 but between austenite and bainite. Same as PLMEM3 but between austenite and martensite. STRC Effective strain rate parameter C. STRC.LT.0.0: load curve id = -STRC STRC.GT.0.0: constant value STRC.EQ.0.0: strain rate NOT active STRP Effective strain rate parameter P. STRP.LT.0.0: load curve id = -STRP STRP.GT.0.0: constant value STRP.EQ.0.0: strain rate NOT active REACT Flag for advanced reaction kinetics input. One additional input card is read. EQ.1.0: Active EQ.0.0: Inactive 0.0 0.0 0.0 0.0 0.0 0.0 0.0 0.0 0.0 TEMPER AUST FERR PEAR BAIN MART GRK GRQR TAU1 GRA GRB EXPA EXPB GRCC *MAT_UHS_STEEL DESCRIPTION BASELINE VALUE Flag for tempering input. One additional input card is read. EQ.1.0: Active EQ.0.0: Inactive If a heating process is initiated at t = 0 this parameters sets the initial amount of austenite in the blank. If heating is activated at t > 0 during a simulation this value is ignored. Note that, AUST + FERR + PEAR + BAIN + MART = 1.0 See AUST for description See AUST for description See AUST for description See AUST for description Growth parameter k (μm2/sec) Grain growth activation energy (J/mol) divided by the universal gas constant. Q/R where R = 8.314472 (J/mol K) Empirical grain growth parameter 𝑐1 describing the function τ(T) Grain growth parameter A Grain growth parameter B. A table of recommended values of GRA and GRB is included in Remark 7. Grain growth parameter a Grain growth parameter b Grain growth parameter with the concentration of non-metals in the blank, weight% of C or N 0.0 0.0 0.0 0.0 0.0 0.0 1011 [9] 3 × 104 [9] 2.08 × 108 [9] [9] [9] 1.0 [9] 1.0 [9] [9] VARIABLE GRCM HEATN TAU2 DESCRIPTION BASELINE VALUE Grain growth parameter with the concentration of metals in the blank, lowest weight% of Cr, V, Nb, Ti, Al. [9] Grain growth parameter n austenite formation for the 1.0 [9] Empirical grain growth parameter 𝑐2 describing the function τ(T) 4.806 [9] FS Manual start temperature Ferrite GT.0.0: Same temperature heating and cooling. is used for LT.0.0: Curve ID: Different start temperatures for cooling and heat- ing given by load curve ID = -FS. First ordinate value is used for cool- ing, last ordinate value for heating. PS BS MS MSIG LCEPS23 Manual start temperature Pearlite. See FS for description. Manual start temperature Bainite. See FS for description. Manual start temperature Martensite. See FS for description. Describes the increase of martensite start temperature for cooling due to applied stress. LT.0: Load Curve ID describes MSIG as a function of triaxiality (pressure / effective stress). MS* = MS + MSIG × 𝜎eff Load Curve ID dependent on plastic strain that scales the activation energy QR2 and QR3. QRx = Qx × CEPS23(𝜀pl) / R BASELINE VALUE Load Curve ID dependent on plastic strain that scales the activation energy QR4. QR4 = Q4 × LCEPS4(𝜀pl) / R ID which describe the martensite the Load Curve increase start of temperature for cooling as a function of plastic strain. MS* = MS + MSIG × 𝜎eff + LCEPS5(𝜀pl) Load curve ID of Vicker hardness vs. hardness temperature calculation. Bainite for Load curve ID of Vicker hardness vs. for Martensite hardness temperature calculation. Critical cooling rate to detect holding phase. Sampling interval for temperature rate monitoring to detect the holding phase Annealing temperature start Annealing temperature end Birth temperature start Young’s modulus material for ghost (quiet) Poisson’s ratio for ghost (quiet) material Thermal expansion coefficient for ghost (quiet) material *MAT_244 VARIABLE LCEPS4 LCEPS5 LCH4 LCH5 DTCRIT TSAMP TASTART TAEND TLSTART EGHOST PGHOST AGHOST Discussion: The phase distribution during cooling is calculated by solving the following rate equation for each phase transition 𝑋̇𝑘 = 𝑔𝑘(𝐺, 𝐶, 𝑇𝑘, 𝑄𝑘)𝑓𝑘(𝑋𝑘), 𝑘 = 2,3,4 where 𝑔𝑘 is a function, taken from Li et al., dependent on the grain number G, the chemical composition C, the temperature T and the activation energy Q. Moreover, the function f is dependent on the actual phase 𝑋𝑘 = 𝑥𝑘/𝑥eq 0.4(𝑋𝑘−1)(1 − 𝑋𝑘)0.4𝑋𝑘, The true amount of martensite, i.e., 𝑘 = 5, is modelled by using the true amount of the austenite left after the bainite phase: 𝑓𝑘(𝑋𝑘) = 𝑋𝑘 𝑘 = 2,3,4 𝑥5 = 𝑥1[1 − 𝑒−𝛼(MS−𝑇)], where 𝑥1 is the true amount of austenite left for the reaction, 𝛼 is a material dependent constant and MS is the start temperature of the martensite reaction. The start temperatures are automatically calculated based on the composition: 1. Ferrite, FS = 1185 − 203 × √C − 15.2 × Ni + 44.7 × Si + 104 × V + 31.5 × Mo + 13.1 × W − 30 × Mn − 11 × Cr − 20 × Cu + 700 × P + 400 × Al + 120 × As + 400 × Ti 2. Pearlite, PS = 996 − 10.7 × Mn − 16.9 × Ni + 29 × Si + 16.9 × Cr + 290 × As + 6.4 × W 3. Bainite, BS = 910 − 58 × C − 35 × Mn − 15 × Ni − 34 × Cr − 41 × Mo 4. Martensite, MS = 812 − 423 × C − 30.4 × Mn − 17.7 × Ni − 12.1 × Cr − 7.5 × Mo + 10 × Co − 7.5 × Si where the element weight values are input on Cards 2 through 4. The automatic start temperatures are printed to the messag file and if they are not accurate enough you can manually set them in the input deck (must be set in absolute temperature, Kelvin). If HEAT > 0, the temperature FSnc (ferrite without C) is also echoed. If the specimen exceeds that temperature all ferrite that is left is instantaneous transformed to austenite. Remarks: 1. History Variables. History variables 1 through 8 include the different phases, the Vickers hardness, the yield stress and the ASTM grain size number. Set NEIPS = 8 (shells) or NEIPH = 8 (solids) on *DATABASE_EXTENT_BINARY. History Variable 1 2 3 4 5 6 7 8 Description Amount austenite Amount ferrite Amount pearlite Amount bainite Amount martensite Vickers hardness Yield stress grain size ASTM number (a low value means large grains and vice versa) 2. Excluding Phases. To exclude a phase from the simulation, set the PHASE parameter accordingly. 3. STRC and STRP. Note that both strain rate parameters must be set to include the effect. It is possible to use a temperature dependent load curve for both parameters simultaneously or for one parameter keeping the other constant. 4. TUNIT. TUNIT is time units per hour and is only used for calculating the Vicker Hardness, as default it is assumed that the time unit is seconds. If other time unit is used, for example milliseconds, then TUNIT must be changed to TUNIT = 3.6 × 106 5. TSF. The thermal speedup factor TSF of *CONTROL_THERMAL_SOLVER is used to scale reaction kinetics and hardness calculations in this material model. On the other hand, strain rate dependent properties are not scaled by TSF. 6. CRSH. With the CRSH = 1 option it is now possible to transfer the material properties from a hot stamping simulation (CRSH = 0) into another simulation. The CRSH = 1 option reads a dynain file from a simulation with CRSH = 0 and keeps all the history variables (austenite, ferrite, pearlite, bainite, martensite, etc) constant. This will allow steels with inhomogeneous strength to be ana- lysed in, for example, a crash simulation. The speed with the CRSH = 1 option is comparable with *MAT_024. Note that for keeping the speed the tempera- ture used in the CRSH simulation should be constant and the thermal solver should be inactive. 7. HEAT. When HEAT is activated the re-austenitization and grain growth algorithms are also activated. The grain growth is activated when the tempera- ture exceeds a threshold value that is given by 𝑇 = 𝐴 − log10[(GRCM)𝑎(GRCC)𝑏] and the rate equation for the grain growth is, 𝑔̇ = 𝑅𝑇. − 2𝑔 The rate equation for the phase re-austenitization is given in Oddy (1996) and is here mirrored 𝑥̇𝑎 = 𝑛 [ln ( 𝑥𝑒𝑢 𝑥𝑒𝑢 − 𝑥𝑎 𝑛−1 )] [ 𝑥𝑒𝑢 − 𝑥𝑎 𝜏(𝑇) ] where n is the parameter HEATN. The temperature dependent function 𝜏(𝑇) is given from Oddy as 𝜏(𝑇) = 𝑐1(𝑇 − 𝑇𝑠)𝑐2. The empirical parameters 𝑐1 and 𝑐2 are calibrated in Oddy to 2.06 × 108 and 4.806 respectively. Note that 𝜏 above given in seconds. Recommended values for GRA and GRB are given in the following table. Compound Metal Non-metal GRA Cr23C6 V4C3 TiC NbC Mo2C Nb(CN) VN AlN NbN TiN Cr V Ti Nb Mo Nb V Al Nb Ti C C0.75 C C0.7 C (CN) N N N N 5.90 5.36 2.75 3.11 5.0 2.26 3.46 + 0.12%Mn 1.03 4.04 0.32 GRB 7375 8000 7000 7520 7375 6770 8330 6770 10230 8000 8. Using the Table Capability for Temperature Dependence of Young’s Modulus. Use *DEFINE_TABLE_2D and set the abscissa value equal to 1 for the austenite YM-curve, equal to 2 for the ferrite YM-curve, equal to 3 for the pearlite YM curve, equal to 4 for the bainite YM-curve and finally equal to 5 for the martensite YM-curve. If you use the PHASE option you only need to define the curves for the included phases, but you can define all five. LS-DYNA uses the number 1-5 to get the right curve for the right phase. The total YM is calcu- lated by a linear mixture law: YM = YM1 × PHASE1 + ⋯ + YM5 × PHASE5. For example: *DEFINE_TABLE_2D $ The number before curve id:s define which phase the curve $ will be applied to. 1 = Austenite, 2 = Ferrite, 3 = Pearlite, $ 4 = Bainite and 5 = Martensite. 1000 0.0 0.0 1.0 100 2.0 200 3.0 300 4.0 400 5.0 500 $ $ Define curves 100 - 500 *DEFINE_CURVE $ Austenite Temp (K) - YM-Curve (MPa) 100 0 1.0 1.0 1300.0 50.E+3 223.0 210.E+3 9. Using the Table Capability for Latent Heat. When using a table ID for the latent heat (LAT1) you can describe all phase transition individually. Use *DE- FINE_TABLE_2D and set the abscissa values to the corresponding phase transi- tion number. That is, 2 for the austenite to ferrite, 3 for the austenite to pearlite, 4 for the austenite to bainite and 5 for the austenite to martensite. Remark 8 demonstrates the form a correct table definition. If a curve is missing, the cor- responding latent heat for that transition will be set to zero. Also, when a table is used the LAT2 is ignored. If HEAT > 0 you also have the option to include latent heat for the transition back to Austenite. This latent heat curve is marked as 1 in the table definition of LAT1. 10. Using the Table Capability for Thermal Expansion. When using a table ID for the thermal expansion you can specify the expansion characteristics for each phase. That is, you can have a curve for each of the 5 phases (austenite, ferrite, pearlite, bainite, and martensite). The input is identical to the above table defi- nitions. The table must have the abscissa values between 1 and 5 where the number correspond to phase 1 to 5. To exclude one phase from influencing the thermal expansion you simply input a curve that is zero for that phase or even easier, exclude that phase number in the table definition. For example, to ex- clude the bainite phase you only define the table with curves for the indices 1, 2, 3 and 5. 11. TEMPER. Tempering is activated by setting TEMPER to 1. When active the default hardness calculation for bainite and martensite is altered to use an in- cremental update formula. The total hardness is given by ∑ HV𝑖 × 𝑥𝑖 . When holding phases are detected the hardness for Bainite and Martensite is updated according to 𝑖=1 HV4 𝑛+1 = HV5 𝑛+1 = 𝑥4 𝑛+1 HV4 𝑥4 𝑥5 𝑛+1 HV5 𝑥5 𝑛 + 𝑛 + ∆𝑥4 𝑛+1 ℎ4(𝑇), 𝑥4 ∆𝑥5 𝑛+1 ℎ5(𝑇), 𝑥5 ∆𝑥4 = 𝑥4 𝑛+1 − 𝑥4 𝑛 ∆𝑥5 = 𝑥5 𝑛+1 − 𝑥5 𝑛 We detect the holding phase for Bainite and Martensite when the temperature is in the appropriate range and if average temperature rate is below DTCRIT. 𝑛 + The average temperature rate is calculated as 𝑛 + ∆𝑡. The average temperature and time are updated until ∣𝑇̇∣∆𝑡 and 𝑡tresh 𝑡tresh ≥ 𝑡samp. where the 𝑇tresh 𝑛+1 = 𝑇tresh 𝑛+1 = 𝑡tresh 𝑇tresh 𝑡tresh 12. CWM (Welding). When computational welding mechanics is activated with CWM = 1 the material can be defined to be initially in a quiet state. In this state the material (often referred to as ghost material) has thermo-mechanical proper- ties defined by an additional card. The material is activated when the tempera- ture reaches the birth temperature. See MAT_CWM (MAT_270) for a detailed description. 13. LCTRE (Transformation Induced Strains). Transformation induced strains can be included with a load curve LCTRE as a function of temperature. The load curve represents the difference between the hard phases and the austenite phase in the dilatometer curves. Therefore, positive curve values result in a negative transformation strain for austenitization and a positive transformation strain for the phase transformation from austenite to one of the hard phases. References: 1. Numisheet 2008 Proceedings, The Numisheet 2008 Benchmark Study, Chapter 3, Benchmark 3, Continuous Press Hardening, Interlaken, Switzerland, Sept. 2008. 2. P. Akerstrom and M. Oldenburg, “Austenite Decomposition During Press hardening of a Boron Steel – Computer Simulation and Test”, Journal of Mate- rial processing technology, 174 (2006), pp399-406. 3. M.V Li, D.V Niebuhr, L.L Meekisho and D.G Atteridge, “A Computatinal model for te prediction of steel hardenability”, Metallurgical and materials transactions B, 29B, 661-672, 1998. 4. D.F. Watt, “An Algorithm for Modelling Microstructural Development in Weld heat-Affected Zones (Part A) Reaction Kinetics”, Acta metal. Vol. 36., No. 11, pp. 3029-3035, 1988. 5. ThyssenKrupp Steel, “Hot Press hardening Manganese-boron Steels MBW”, product information Manganese-boron Steels, Sept. 2008. 6. Malek Naderi, “Hot Stamping of Ultra High Strength Steels”, Doctor of Engineering Dissertation, Technical University Aachen, Germany, 2007. 7. P. Akerstrom, “Numerical Implementation of a Constitutive model for Simulation of Hot Stamping”, Division of Solid Mechanics, Lulea University of technology, Sweden. 8. Malek Naderi, “A numerical and Experimental Investigation into Hot Stamping of Boron Alloyed Heat treated Steels”, Steel research Int. 79 (2008) No. 2. 9. A.S. Oddy, J.M.J. McDill and L. Karlsson, “Microstructural predictions including arbitrary thermal histories, reaustenitization and carbon segregation effects” (1996). Boron steel composition from the literature: Element HAZ code Akerstrom (2) Naderi (8) ThyssenKrupp(4) (max amount) B C Co Mo Cr Ni Mn Si V W Cu P Al As Ti S 0.168 0.036 0.255 0.015 1.497 0.473 0.026 0.025 0.012 0.020 0.003 0.23 0.211 1.25 0.29 0.003 0.230 0.160 1.18 0.220 0.005 0.250 0.250 0.250 1.40 0.400 0.013 0.015 0.025 0.003 0.040 0.001 0.05 0.010 *MAT_PML_OPTIONTROPIC_ELASTIC This is Material Type 245. This is a perfectly-matched layer (PML) material for orthotropic or anisotropic media, to be used in a wave-absorbing layer adjacent to an orthotropic/anisotropic material (*MAT_{OPTION}TROPIC_ELASTIC) in order to simulate wave propagation in an unbounded ortho/anisotropic medium. This material is a variant of MAT_PML_ELASTIC (MAT_230) and is available only for solid 8-node bricks follow *MAT_{OPTION}TROPIC_ELASTIC as shown below. See the variable descriptions and Remarks section of *MAT_{OPTION}TROPIC_ELASTIC (*MAT_002) for further details. input cards exactly type 2). (element The Available options include: ORTHO ANISO such that the keyword cards appear: *MAT_PML_ORTHOTROPIC_ELASTIC or MAT_245 (4 cards follow) *MAT_PML_ANISOTROPIC_ELASTIC or MAT_245_ANISO (5 cards follow) Orthotropic Card 1. Card 1 format used for ORTHO keyword option. Card 1 1 Variable MID 2 RO Type A8 F 3 EA F 4 EB F 5 EC F 6 7 8 PRBA PRCA PRCB F F F Orthotropic Card 2. Card 2 format used for ORTHO keyword option. Card 2 1 2 3 4 Variable GAB GBC GCA AOPT Type F F F F 5 G F 6 7 8 SIGF Anisotropic Card 1. Card 1 format used for ANISO keyword option. Card 1 1 Variable MID 2 RO 3 4 5 6 7 8 C11 C12 C22 C13 C23 C33 Type A8 F F F F F F F Anisotropic Card 2. Card 2 format used for ANISO keyword option. Card 2 1 2 3 4 5 6 7 8 Variable C14 C24 C34 C44 C15 C25 C35 C45 Type F F F F F F F F Anisotropic Card 3. Card 3 format used for ANISO keyword option. Card 3 1 2 3 4 5 6 7 8 Variable C55 C16 C26 C36 C46 C56 C66 AOPT Type F F F F F F Card 4 Variable 1 XP Type F Card 5 Variable 1 V1 Type F 2 YP F 2 V2 F 3 ZP F 3 V3 F 4 A1 F 4 D1 F 5 A2 F 5 D2 F 6 A3 F 6 D3 F F 7 MACF I 7 F 8 8 BETA REF F Remarks: 1. A layer of this material may be placed at a boundary of a bounded domain to simulate unboundedness of the domain at that boundary: the layer absorbs and attenuates waves propagating outward from the domain, without any signifi- cant reflection of the waves back into the bounded domain. The layer cannot support any static displacement. 2. It is assumed the material in the bounded domain near the layer is, or behaves like, a linear ortho/anisotropic material. The material properties of the layer should be set to the corresponding properties of this material. 3. The layer should form a cuboid box around the bounded domain, with the axes of the box aligned with the coordinate axes. Various faces of this box may be open, as required by the geometry of the problem, e.g., for a half-space prob- lem, the “top” of the box should be open. 4. Internally, LS-DYNA will partition the entire PML into regions which form the “faces”, “edges” and “corners” of the above cuboid box, and generate a new material for each region. This partitioning will be visible in the d3plot file. The user may safely ignore this partitioning. 5. The layer should have 5 - 10 elements through its depth. Typically, 5 - 6 elements are sufficient if the excitation source is reasonably distant from the layer, and 8 - 10 elements if it is close. The size of the elements should be simi- lar to that of elements in the bounded domain near the layer, and should be small enough to sufficiently discretize all significant wavelengths in the prob- lem. 6. The nodes on the outer boundary of the layer should be fully constrained. 7. The stress and strain values reported by this material do not have any physical significance. *MAT_PML_NULL This is Material Type 246. This is a perfectly-matched layer (PML) material with a pressure fluid constitutive law computed using an equation of state, to be used in a wave-absorbing layer adjacent to a fluid material (*MAT_NULL with an EOS) in order to simulate wave propagation in an unbounded fluid medium. Only *EOS_LINEAR_- POLYNOMIAL and *EOS_GRUNEISEN are allowed with this material. See the Remarks section of *MAT_NULL (*MAT_009) for further details. Accurate results are to be expected only for the case where the EOS presents a linear relationship between the pressure and volumetric strain. This material is a variant of MAT_PML_ELASTIC (MAT_230) and is available only for solid 8-node bricks (element type 2). 4 5 6 7 8 Card 1 Variable MID 2 RO 3 MU Type A8 F F Default none none 0.0 VARIABLE DESCRIPTION Material identification. A unique number or label not exceeding 8 characters must be specified. Mass density. Dynamic viscosity coefficient MID RO MU Remarks: 1. A layer of this material may be placed at a boundary of a bounded domain to simulate unboundedness of the domain at that boundary: the layer absorbs and attenuates waves propagating outward from the domain, without any signifi- cant reflection of the waves back into the bounded domain. The layer cannot support any static displacement. 2. It is assumed the material in the bounded domain near the layer is, or behaves like, an linear fluid material. The material properties of the layer should be set to the corresponding properties of this material. 3. The layer should form a cuboid box around the bounded domain, with the axes of the box aligned with the coordinate axes. Various faces of this box may be open, as required by the geometry of the problem, e.g., for a half-space prob- lem, the “top” of the box should be open. 4. Internally, LS-DYNA will partition the entire PML into regions which form the “faces”, “edges” and “corners” of the above cuboid box, and generate a new material for each region. This partitioning will be visible in the d3plot file. The user may safely ignore this partitioning. 5. The layer should have 5-10 elements through its depth. Typically, 5-6 elements are sufficient if the excitation source is reasonably distant from the layer, and 8- 10 elements if it is close. The size of the elements should be similar to that of elements in the bounded domain near the layer, and should be small enough to sufficiently discretize all significant wavelengths in the problem. 6. The nodes on the outer boundary of the layer should be fully constrained. 7. The stress and strain values reported by this material do not have any physical significance. *MAT_PHS_BMW This is Material Type 248. This model is intended for hot stamping processes with phase transformation effects. It is available for shell elements only and is based on Material Type 244 (*MAT_UHS_STEEL). As compared with Material Type 244 Material Type 248 features: 1. 2. 3. a more flexible choice of evolution parameters, an approach for transformation induced strains, and a more accurate density calculation of individual phases. Thus the metal physical effects can be taken into account calculating the volume fractions of ferrite, pearlite, bainite and martensite for fast supercooling as well as for slow cooling conditions. Furthermore, this material model features cooling-rate dependence for several of its more crucial material parameters in order to accurately calculate the Time-Temperature-Transformation diagram dynamically. A detailed description can be found in Hippchen et al. [2013] and Hippchen [2014]. NOTE 1: For this material “weight%” means “ppm × 10-4”. NOTE 2: For this material the phase frac- tions are calculated in volume per- cent (vol%). Card 1 1 Variable MID Type I 2 RO F 3 E F 4 PR F Defaults none none none none 3600 5 6 7 8 TUNIT TRIP PHASE HEAT F I 0 I 0 I Card 2 1 2 3 4 5 6 7 8 Variable LCY1 LCY2 LCY3 LCY4 LCY5 C_F C_P C_B Type I I I I I F F F Defaults none none none none none 0.0 0.0 0.0 Card 3 Variable Type 1 C F 2 Co F 3 Mo F 4 Cr F 5 Ni F 6 Mn F 7 Si F 8 V F Defaults 0.0 0.0 0.0 0.0 0.0 0.0 0.0 0.0 Card 4 Variable Type 1 W F 2 Cu F 3 P F 4 Al F 5 As F 6 Ti F 7 B F 8 Defaults 0.0 0.0 0.0 0.0 0.0 0.0 0.0 Card 5 1 2 3 4 5 6 7 8 Variable Type Defaults TABRHO TREF LAT1 LAT5 TABTH I F F F I none none 0.0 0.0 none Card 6 1 2 3 4 5 6 7 8 Variable QR2 QR3 QR4 ALPHA GRAIN TOFFE TOFPE TOFBA Type F F F F F F F F Defaults 0.0 0.0 0.0 0.0 0.0 0.0 0.0 0.0 Card 7 1 2 3 4 5 6 7 8 Variable PLMEM2 PLMEM3 PLMEM4 PLMEM5 STRC STRP Type F F F F F F Defaults 0.0 0.0 0.0 0.0 0.0 0.0 Card 8 Variable 1 FS Type F 2 PS F 3 BS F 4 5 6 7 8 MS MSIG LCEPS23 LCEPS4 LCEPS5 F F I I I Defaults 0.0 0.0 0.0 0.0 none none none none Card 9 1 2 3 4 5 6 7 8 Variable LCH4 LCH5 DTCRIT TSAMP ISLC IEXTRA Type Defaults I 0 I 0 F F 0.0 0.0 I 0 I Card 10 1 2 3 4 5 6 7 8 Variable ALPH_M N_M PHI_M PSI_M OMG_F PHI_F PSI_F CR_F Type F F F F F F F F Defaults 0.0428 0.191 0.382 2.421 0.41 0.4 0.4 0.0 Card 11 1 2 3 4 5 6 7 8 Variable OMG_P PHI_P PSI_P CR_P OMG_B PHI_B PSI_B CR_B Type F F F F F F F F Defaults 0.32 0.4 0.4 0.0 0.29 0.4 0.4 0.0 Heat Card 1. Additional Card for HEAT ≠ 0. Card 12 1 2 3 4 5 6 7 8 Variable AUST FERR PEAR BAIN MART GRK GRQR TAU1 Type F F F F F F F F Default 0.0 0.0 0.0 0.0 0.0 0.0 0.0 2.08E+8 Heat Card 2. Additional Card for HEAT ≠ 0. Card 13 1 2 3 4 5 6 7 8 Variable GRA GRB EXPA EXPB GRCC GRCM HEATN TAU2 Type F F F F F F F F Default 3.11 7520. 1.0 1.0 none none 1.0 4.806 Extra Card 1. Additional Card for IEXTRA = 1. Card 14 1 2 3 4 5 6 7 8 Variable FUNCA FUNCB FUNCM TCVUP TCVLO CVCRIT TCVSL Type F F F F F F F Default 0.0 0.0 0.0 0.0 0.0 0.0 0.0 Extra Card 2. Additional Card for IEXTRA = 2. Card 15 1 2 3 4 5 6 7 8 Variable EPSP EXPON Type F F Default 0.0 0.0 VARIABLE DESCRIPTION BASELINE VALUE MID RO Material ID, a unique number has to be chosen. Material density at room temperature (necessary for calculating transformation induced strains) 7830 Kg/m3 E Youngs’ modulus: 100.e+09 Pa [1] GT.0.0: constant value is used LT.0.0: LCID or TABID. Temperature dependent Young’s modulus given by load curve or table ID = -E. When using a table to describe the Young’s modulus see Remark 10 for more infor- mation. VARIABLE DESCRIPTION BASELINE VALUE PR Poisson’s ratio: 0.30 [1] 3600. 0 0 TUNIT TRIP PHASE GT.0.0: constant value is used LT.0.0: LCID or TABID. Temperature dependent Poisson’s ratio giv- en by load curve or table ID = - PR. The table input is de- scribed in Remark 10. Number of time units per hour. Default is seconds, that is 3600 time units per hour. It is used only for hardness calculations. Flag to activate (0) or deactivate (1) trip effect calculation. Switch to exclude middle phases from the simulation. EQ.0: all phases active (default) EQ.1: pearlite and bainite active EQ.2: bainite active EQ.3: ferrite and pearlite active EQ.4: ferrite and bainite active EQ.5: no active middle phases (only austenite → martensite) HEAT Heat flag as in MAT_244, see there for details. EQ.0: Heating is not activated. EQ.1: Heating is activated. EQ.2: Automatic switching between cooling and heating. LT.0: Switch between cooling and heating is defined by a time de- id pendent ABS(HEAT). load curve with LCY1 LCY2 LCY3 LCY4 LCY5 C_F C_P C_B C Co Mo *MAT_PHS_BMW DESCRIPTION BASELINE VALUE Load curve or Table ID for austenite hardening. if LCID input yield stress versus effective plastic strain. if TABID.GT.0: 2D table. Input temperatures as table values and hardening curves as targets for those temperatures if TABID.LT.0: 3D table. Input temperatures as main table values and strain rates as values for the sub tables, and hardening curves as targets for those strain rates. Load curve or Table ID for ferrite. See LCY1 for description. Load curve or Table ID for pearlite. See LCY1 for description. Load curve or Table ID for bainite. See LCY1 for description. Load curve or Table ID for martensite. See LCY1 for description. for ferrite Alloy dependent factor 𝐶𝑓 (controls the alloying effects beside of Boron time-temperature- the transformation start line of ferrite). on Alloy dependent factor 𝐶𝑝 for pearlite . Alloy dependent factor 𝐶𝑏 for bainite . Carbon [weight %] Cobolt [weight %] Molybdenum [weight %] [5] 0.23 [2, 4] 0.0 [2, 4] 0.0 [2, 4] VARIABLE DESCRIPTION BASELINE VALUE Cr Ni Mn Si V W Cu P Al As Ti Β TABRHO TREF LAT1 Chromium [weight %] Nickel [weight %] Manganese [weight %] Silicon [weight %] Vanadium [weight %] Tungsten [weight %] Copper [weight %] Phosphorous [weight %] Aluminium [weight %] Arsenic [weight %] Titanium [weight %] Boron [weight %] for definition and Table temperature densities. Needed for calculation of transformation induced strains. dependent phase temperature Reference thermal expansion (only necessary for thermal expansion calculation with the secant method). for 0.21 [2, 4] 0.0 [2, 4] 1.25 [2, 4] 0.29 [2, 4] 0.0 [2, 4] 0.0 0.0 0.013 0.0 0.0 0.0 0.0 293.15 Latent heat for the decomposition of austenite into ferrite, pearlite and bainite. GT.0.0: Constant value 590.e+06 J/m3 [2] LT.0.0: Curve ID or Table ID: See infor- for more remark 11 mation. 640.e+06 J/m3 [2] *MAT_248 VARIABLE LAT5 DESCRIPTION Latent heat for the decomposition of austenite into martensite. GT.0.0: Constant value LT.0.0: Curve ID: Note that LAT 5 is ignored if a Table ID is used in LAT1. TABTH Table definition for thermal expansion coefficient. for more See remarks information how to input this table. QR2 QR3 QR4 ALPHA GT.0: A for table instantaneous thermal expansion (TREF is ig- nored). LT.0: A table with thermal expansion with reference to TREF. energy divided by Activation the universal gas constant for the diffusion reaction of the austenite-ferrite reaction: Q2/R. R = 8.314472 [J/mol K]. energy divided by the Activation universal gas constant for the diffusion reaction austenite-pearlite the reaction: Q3/R. R = 8.314472 [J/mol K]. for energy divided by Activation the universal gas constant for the diffusion reaction for the austenite-bainite reaction: Q4/R. R = 8.314472 [J/mol K]. for Material constant the martensite phase. A value of 0.011 means that 90% of the available austenite is transformed into martensite at 210 degrees below the , whereas a value 99.9% 0.033 means transformation. temperature start of a 10324 K [3] = (23000 cal/mole) × (4.184 J/cal) / (8.314 J/mole/K) 13432. K [3] 15068. K [3] 0.011 GRAIN ASTM grain size number 𝐺 for austenite, usually a number between 7 and 11. 6.8 DESCRIPTION BASELINE VALUE VARIABLE TOFFE TOFPE TOFBA PLMEM2 PLMEM3 PLMEM4 PLMEM5 STRC Number of degrees that the ferrite is bleeding over into the pearlite reaction: 𝑇off,𝑓 . Number of degrees that the pearlite is bleeding over into the bainite reaction: 𝑇off,𝑝. Number of degrees that the bainite is the martensite into bleeding over reaction: 𝑇off,𝑏. Memory coefficient for the plastic strain that is carried over from the austenite. A value of 1 means that all plastic strains from austenite is transferred to the ferrite phase and a value of 0 means that nothing is transferred. Same as PLMEM2 but between austenite and pearlite. Same as PLMEM2 but between austenite and bainite. Same as PLMEM3 but between austenite and martensite. Cowper parameter 𝐶. and Symonds strain rate STRC.LT.0.0: load curve id = -STRC STRC.GT.0.0: constant value STRC.EQ.0.0: strain rate NOT active STRP Cowper parameter P. and Symonds strain rate STRP.LT.0.0: load curve id = -STRP STRP.GT.0.0: constant value STRP.EQ.0.0: strain rate NOT active 0.0 0.0 0.0 0.0 0.0 0.0 0.0 0.0 0.0 VARIABLE DESCRIPTION BASELINE VALUE FS Manual start temperature ferrite, 𝐹𝑆. GT.0.0: Same temperature is used for heating and cooling. LT.0.0: Curve ID: Different start temperatures for cooling and heating given by load curve ID = -FS. First ordinate value is used for cooling, last ordinate value for heating. Manual start temperature pearlite, 𝑃𝑆. See FS for description. Manual start temperature bainite, 𝐵𝑆. See FS for description. Manual start temperature martensite, 𝑀𝑆. See FS for description. Describes the increase of martensite start temperature for cooling due to applied stress. LT.0: Load Curve ID describes MSIG as a function of triaxiality (pressure / effective stress). MS* = MS + MSIG × 𝜎eff Load Curve ID dependent on plastic strain that scales the activation energy QR2 and QR3. QRn = Qn × LCEPS23(𝜀pl)/𝑅 Load Curve ID dependent on plastic strain that scales the activation energy QR4. QR4 = Q4 × LCEPS4(𝜀pl)/𝑅 PS BS MS MSIG LCEPS23 LCEPS4 VARIABLE LCEPS5 LCH4 LCH5 DTCRIT TSAMP ISLC DESCRIPTION BASELINE VALUE ID which describe the martensite the Load Curve increase start of temperature for cooling as a function of plastic strain. MS* = MS + MSIG × 𝜎eff + LCEPS5(𝜀pl) Load curve ID of Vickers hardness vs. temperature hardness calculation. bainite for Load curve ID of Vickers hardness vs. temperature for martensite hardness calculation. Critical cooling rate to detect holding phase. Sampling interval for temperature rate monitoring to detect the holding phase for Flag parameters on Cards 10 and 11. definition of evolution EQ.0.0: All 16 parameters on Cards 10 and 11 are constant values. EQ.1.0: PHI_F, CR_F, PHI_P, CR_P, PHI_B, and CR_B are load curves defining values as functions of cooling rate. The remaining 10 paramters on Cards 10 and 11 are constant values. EQ.2.0: All 16 parameters on Cards 10 and 11 are load curves defin- ing values as functions of cool- ing rate. IEXTRA Flag to read extra cards ALPH_M Martensite evolution parameter 𝛼𝑚 N_M PHI_M Martensite evolution parameter 𝑛𝑚 Martensite evolution parameter 𝜑𝑚 0.0428 0.191 0.382 PSI_M OMG_F PHI_F PSI_F CR_F OMG_P PHI_P PSI_P CR_P OMG_B PHI_B PSI_B CR_B *MAT_PHS_BMW DESCRIPTION BASELINE VALUE Martensite evolution exponent 𝜓𝑚, 𝜓𝑚 < 0 then 𝜓𝑚 = ∣𝜓𝑚∣(2 − 𝜍𝑎) if Ferrite grain size factor 𝜔𝑓 (mainly controls the alloying effect of Boron on the time-temperature-transformation start line of ferrite) Ferrite evolution parameter 𝜑𝑓 (controls the incubation time till 1vol% of ferrite is built) Ferrite evolution parameter 𝜓𝑓 (controls the time till 99vol% of ferrite is built without effect on the incubation time) evolution parameter Ferrite 𝐶𝑟,𝑓 (retardation coefficient to influence the kinetics of phase transformation of ferrite, should be determined at slow cooling in conditions, can also be defined dependency to the cooling rate) Pearlite grain size factor 𝜔𝑝 Pearlite evolution parameter 𝜑𝑝 PHI_F for description) Pearlite evolution parameter 𝐶𝑟,𝑝 Bainite grain size factor 𝜔𝑏 Bainite evolution parameter 𝜑𝑏 Bainite evolution parameter 𝜓𝑏 Bainite evolution parameter 𝐶𝑟,𝑏 CR_F for description) (see 2.421 0.41 0.4 0.4 0.0 0.32 0.4 0.4 0.0 0.32 0.4 0.4 0.0 DESCRIPTION BASELINE VALUE VARIABLE AUST FERR PEAR BAIN MART GRK GRQR TAU1 GRA GRB EXPA EXPB GRCC GRCM If a heating process is initiated at t = 0 this parameters sets the initial amount of austenite in the blank. If heating is activated at t > 0 during a simulation this value is ignored. Note that, AUST + FERR + PEAR + BAIN + MART = 1.0 See AUST for description See AUST for description See AUST for description See AUST for description Growth parameter k (μm2/sec) Grain growth activation energy (J/mol) divided by the universal gas constant. Q/R where R = 8.314472 (J/mol K) Empirical grain growth parameter 𝑐1 describing the function τ(T) Grain growth parameter A Grain growth parameter B. A table of recommended values of GRA and GRB is included in Remark 7 of *MAT_244. Grain growth parameter 𝑎 Grain growth parameter 𝑏 Grain growth parameter with the concentration of non metals in the blank, weight% of C or N Grain growth parameter with the concentration of metals in the blank, lowest weight% of Cr, V, Nb, Ti, Al. 0.0 0.0 0.0 0.0 0.0 1.0E+11[9] 3.0E+4[9] 2.08E+8 [9] [9] [9] 1.0 [9] 1.0 [9] [9] [9] 1.0[9] HEATN Grain growth parameter 𝑛 for austenite formation the BASELINE VALUE Empirical grain growth parameter 𝑐2 describing the function τ(T) 4.806[9] ID of a saturation approach) *DEFINE_FUNCTION stress A for (Hockett-Sherby ID of a *DEFINE_FUNCTION for initial yield stress B (Hockett-Sherby approach) ID of a saturation approach) *DEFINE_FUNCTION rate M for (Hockett-Sherby Upper temperature for determination of average cooling velocity Lower temperature for determination of average cooling velocity Critical cooling velocity. If the average cooling velocity is smaller or equal CVCRIT, the cooling rate at TCVSL is used. Temperature for determination of cooling velocity for small cooling velocities. Plastic strain in Hockett-Sherby approach Exponent in Hockett-Sherby approach *MAT_248 VARIABLE TAU2 FUNCA FUNCB FUNCM TCVUP TCVLO CVCRIT TCVSL EPSP EXPON Remarks: 1. Start Temperatures. Start temperatures for ferrite, pearlite, bainite, and martensite can be defined manually via FS, PS, BS, and MS. Or they are initially defined using the following composition equations: 𝐹𝑆 = 273.15 + 912 − 203 × √C − 15.2 × Ni + 44.7 × Si + 104 × V + 31.5 × Mo + 13.1 × W − 30 × Mn − 11 × Cr − 20 × Cu + 700 × P + 400 × Al + 120 × As + 400 𝑃𝑆 = 273.15 + 723 − 10.7 × Mn − 16.9 × Ni + 29 × Si + 16.9 × Cr + 290 × As + 6.4 × W 𝐵𝑆 = 273.15 + 637 − 58 × C − 35 × Mn − 15 × Ni − 34 × Cr − 41 × Mo 𝑀𝑆 = 273.15 + 539 − 423 × C − 30.4 × Mn − 17.7 × Ni − 12.1 × Cr − 7.5 × Mo + 10 × Co − 7.5 × Si 2. Martensite Phase Evolution. Martensite phase evolution according to Lee et al. [2008, 2010] if PSI_M > 0: d𝜉𝑚 d𝑇 = α𝑚(𝑀𝑆 − 𝑇)𝑛𝜉𝑚 𝜑𝑚(1 − 𝜉𝑚)𝜓𝑚 Martensite phase evolution according to Lee et al. [2008, 2010] with extension by Hippchen et al. [2013] if PSI_M < 0: d𝜉𝑚 d𝑇 = α𝑚(𝑀𝑆 − 𝑇)𝑛𝜉𝑚 𝜑𝑚(1 − 𝜉𝑚)𝜓𝑚(2−𝜁𝑎) 3. Phase Change Kinetics for Ferrite, Pearlite and Bainite. d𝜉𝑓 d𝑡 = 2𝜔𝑓 𝐺 exp (− 𝑄𝑓 𝑅𝑇 ) 𝐶𝑓 (𝐹𝑆 − 𝑇)3 𝜓𝑓 𝜉𝑓 𝜉 𝜑𝑓 (1−𝜉𝑓 )(1 − 𝜉𝑓 ) 2) exp(𝐶𝑟,𝑓 𝜉𝑓 for 𝐹𝑆 ≥ 𝑇 ≥ (𝑃𝑆 − 𝑇off,𝑓 ) d𝜉𝑝 d𝑡 = 2𝜔𝑝𝐺 exp (− 𝑄𝑝 𝑅𝑇 ) 𝐶𝑝 (𝑃𝑆 − 𝑇)3 𝜓𝑝𝜉𝑝 𝜉 𝜑𝑝(1−𝜉𝑝)(1 − 𝜉𝑝) 2) exp(𝐶𝑟,𝑝𝜉𝑝 for 𝑃𝑆 ≥ 𝑇 ≥ (𝐵𝑆 − 𝑇off,𝑝) d𝜉𝑏 d𝑡 = 2𝜔𝑏𝐺 exp (− 𝑄𝑏 𝑅𝑇 ) 𝐶𝑏 (𝐵𝑆 − 𝑇)2 𝜉 𝜑𝑏(1−𝜉𝑏)(1 − 𝜉𝑏)𝜓𝑏𝜉𝑏 exp(𝐶𝑟,𝑏𝜉𝑏 2) for 𝑀𝑆 ≥ 𝑇 ≥ (𝑀𝑆 − 𝑇off,𝑏) 4. History Variables. History variables of this material model are listed in the following table. To be able to post-process that data, parameters NEIPS (shells) or NEIPH (solids) have to be defined on *DATABASE_EXTENT_BINARY. History Variable Description 1 2 3 4 5 6 7 8 9 10 11 12 13 17 19 25 26 Amount austenite Amount ferrite Amount pearlite Amount bainite Amount martensite Vickers hardness Yield stress ASTM grain size number Young’s modulus Saturation stress A (H-S approach) Initial yield stress B (H-S approach) Saturation rate M (H-S approach) Yield stress of H-S approach 𝜎𝑦 = 𝐴 − (𝐴 − 𝐵) ∙ 𝑒−𝑀∙𝐸𝑃𝑆𝑃𝐸𝑋𝑃𝑂𝑁 Temperature rate Current temperature Plastic strain rate Effective thermal expansion coefficient 5. Choosing/Excluding Phases. To exclude a phase from the simulation, set the PHASE parameter accordingly. 6. Strain Rate Effects. Note that both strain rate parameters (STRC and STRP) must be set to include the effect. It is possible to use a temperature dependent load curve for both parameters simultaneously or for one parameter keeping the other constant. 7. Time Units. TUNIT is time units per hour and is only used for calculating the Vicker Hardness, as default it is assumed that the time unit is seconds. If other time unit is used, for example milliseconds, then TUNIT must be changed to TUNIT = 3.6 × 106 8. Thermal Speedup Factor. The thermal speedup factor TSF of *CONTROL_- THERMAL_SOLVER is used to scale reaction kinetics and hardness calcula- tions in this material model. On the other hand, strain rate dependent properties are not scaled by TSF. 9. Re-austenization and Grant Growth with HEAT Option. When HEAT is activated the re-austenitization and grain growth algorithms are also activated. See MAT_244 for details. 10. Phase Indexed Tables. When using a Table ID for describing the Young’s modulus as dependent on the temperature Use *DEFINE_TABLE_2D and set the abscissa value equal to 1 for the austenite YM-curve, equal to 2 for the fer- rite YM-curve, equal to 3 for the pearlite YM curve, equal to 4 for the bainite YM-curve and finally equal to 5 for the martensite YM-curve. When using the PHASE option only the curves for the included phases are required, but all five phases may be included. The total YM is calculated by a linear mixture law: YM = YM1 × PHASE1 + ⋯ + YM5 × PHASE5 For example: *DEFINE_TABLE_2D $ The number before curve id:s define which phase the curve $ will be applied to. 1 = Austenite, 2 = Ferrite, 3 = Pearlite, $ 4 = Bainite and 5 = Martensite. 1000 0.0 0.0 1.0 100 2.0 200 3.0 300 4.0 400 5.0 500 $ $ Define curves 100 - 500 *DEFINE_CURVE $ Austenite Temp (K) - YM-Curve (MPa) 100 0 1.0 1.0 1300.0 50.E+3 223.0 210.E+3 11. Phase-indexed Latent Heat Table. A Table ID may be specified for the Latent heat (LAT1) to describe each phase change individually. Use *DEFINE_TA- BLE_2D and set the abscissa values to the corresponding phase transition num- ber. That is, 2 for the Austenite – Ferrite, 3 for the Austenite – Pearlite,’4’ for the Austenite – Bainite and 5 for the Austenite – Martensite. See Remark 7 for an example of a correct table definition. If a curve is missing, the corresponding latent heat for that transition will be set to zero. Also, when a table is used the LAT2 is ignored. If HEAT.GT.0 you also have the option to include latent heat for the transition back to Austenite. This latent heat curve is marked as 1 in the table definition of LAT1. 12. Phase-indexed Thermal Expansion Table. Tables are supported for defining different thermal expansion properties for each phase. The input is identical to the above table definitions. The Table must have the abscissa values between 1 and 5 where the number correspond to phase 1 to 5. To exclude one phase from influencing the thermal expansion you simply input a curve that is zero for that phase or even easier, exclude that phase number in the table definition. For example to exclude the bainite phase you only define the table with curves for the indices 1, 2, 3 and 5. 13. Phase-indexed Transformation Induced Strain Properties. Transformation induced strains can be define with a table TABRHO, where densities are de- fined as functions of phase (table abscissas) and temperature (load curves). *MAT_REINFORCED_THERMOPLASTIC This is material type 249. This material model describes a reinforced thermoplastic composite material. The reinforcement is defined as an anisotropic hyper-elastic material with up to three distinguished fiber directions. It can be used to model unidirectional layers as well as woven and non-crimped fabrics. The matrix is modeled with a simple thermal elasto-plastic material formulation. For a composite an additive composition of fiber and matrix stresses is used. Card 1 1 Variable MID Type A8 Card 2 1 2 RO F 2 Variable NFIB AOPT Type I F Card 3 Variable 1 V1 Type F Card 4 1 2 V2 F 2 3 4 5 6 7 8 EM LCEM PRM LCPRM LCSIGY BETA F I F I I F 3 XP F 3 V3 F 3 4 YP F 4 D1 F 4 5 ZP F 5 D2 F 5 6 A1 F 6 7 A2 F 7 8 A3 F 8 D3 MANGL THICK F 6 F 7 F 8 Variable IDF1 ALPH1 EF1 LCEF1 G23_1 G31_1 Type I F F I F Card 5 1 2 3 4 5 6 7 8 Variable G12 LCG12 ALOC12 GLOC12 METH12 Type F Card 6 1 I 2 F 3 F 4 I 5 6 7 8 Variable IDF2 ALPH2 EF2 LCEF2 G23_2 G31_2 Type I Card 7 1 F 2 F 3 I 4 F 5 F 6 7 8 Variable G23 LCG23 ALOC23 GLOC23 METH23 Type F Card 8 1 I 2 F 3 F 4 I 5 6 7 8 Variable IDF3 ALPH3 EF3 LCEF3 G23_3 G31_3 Type I F F I F F The following card is optional Card 9 1 2 3 4 5 6 7 8 Variable POSTV Type F VARIABLE MID 2-1256 (MAT_248) DESCRIPTION Material identification. A unique number or label not exceeding 8 VARIABLE DESCRIPTION RO EM LCEM PR LCPR Density. Young’s modulus of matrix material. Curve ID for Young’s modulus of matrix material versus temperature. With this option active, EM is ignored. Poisson’s ratio for matrix material Curve temperature. With this option active, PR is ignored. for Poisson’s ratio of matrix material versus ID LCSIGY Load curve or table ID for strain hardening of the matrix. IF LCSIGY refers to a curve Input yield stress versus effective plastic strain. IF LCSIGY refers to a table: Input temperatures as table values and hardening curves as targets for those temperatures BETA Parameter for mixed hardening. Set 𝛽 = 0 for pure kinematic hardening and 𝛽 = 1 for pure isotropic hardening. NFIB Number of fiber families to be considered. AOPT *MAT_REINFORCED_THERMOPLASTIC DESCRIPTION Material axes option : EQ.0.0: locally orthotropic with material axes determined by element nodes, as with *DEFINE_COORDI-NATE_- NODES, and then rotated about the shell element nor- mal by the angle MANGL. EQ.2.0: globally orthotropic with material axes determined by vectors defined below, as with *DEFINE_COORDI- NATE_VECTOR. EQ.3.0: locally orthotropic material axes determined by rotatingthe material axes about the element normal by an angle, MANGL, from a line in the plane of the ele- ment defined by the cross product of the vector v with the element normal LT.0.0: the absolute value of AOPT is a coordinate system ID number (CID on *DEFINE_COORDINATE_NODES, *DEFINE_COORDINATE_SYSTEM or *DEFINE_CO- ORDINATE_VECTOR). XP, YP, ZP Coordinates of point 𝐩 for AOPT = 1. A1, A2, A3 Components of vector 𝐚 for AOPT = 2. V1, V2, V3 Components of vector 𝐯 for AOPT = 3. D1, D2, D3 Components of vector 𝐝 for AOPT = 2. MANGL THICK Material angle in degrees for AOPT = 0 and 3, may be overwritten on the element card, see *ELEMENT_SHELL_BETA. Balance thickness changes of the material due to the matrix description by scaling fiber stresses EQ.0: No scaling EQ.1: Scaling IDFi ID for i-th fiber family for post-processing ALPHi Orientation angle 𝛼𝑖 for i-th fiber with respect to overall material direction EFi Young’s modulus for i-th fiber family VARIABLE DESCRIPTION LCEFi G23_i G31_i Gij LCGij Curve ID for stress versus fiber elongation of i-th fiber. With this option active, EFi is ignored. Transversal shear modulus orthogonal to direction of fiber i Transversal shear modulus in direction of fiber i Linear shear modulus for shearing between fiber i and j Curve ID for shear stress versus shearing between of i-th and j-th fiber. With this option active, Gij is ignored. For details see parameter METHij. ALOCij Locking angle (in radians) for shear between fiber families i and j GLOCij Linear shear modulus for shear angles larger than ALOCij METHij Option for shear between fiber i and j : EQ.0: Elastic shear response, curve LCGij defines shear stress vs. scalar product of fibers directions. EQ.1 Elasto-plastic shear response, curve LCGij defines yield shear stress vs. normalized scalar product of fiber di- rections. EQ.2: Elastic shear response, curve LCGij defines shear stress vs. shear angle between fibers given in rad. EQ.3: Elasto-plastic shear response, curve LCGij defines yield shear stress vs. normalized shear angle between fi- bers. EQ.4: Elastic shear response, curve LCGij defines shear stress vs. shear angle between fibers given in rad. This option is a special implementation for non- crimped fabrics, where one of the fiber families corre- sponds to a stitching. EQ.5: Elasto-plastic shear response, curve LCGij defines yield shear stress vs. normalized shear angle between fi- bers. This option is a special implementation for non- crimped fabrics, where one of the fiber families corre- sponds to a stitching. EQ.10: Elastic shear response, curve LCGij defines shear stress vs. shear angle between fibers given in rad. This option is tailored for woven fabrics and guaran- tees a pure shear stress response. *MAT_REINFORCED_THERMOPLASTIC DESCRIPTION EQ.11: Elasto-plastic shear response, curve LCGij defines yield shear stress vs. normalized shear angle. This option is tailored for woven fabrics and guarantees a pure shear stress response POSTV Defines additional history variables that might be useful for post- processing. See remarks below for details. Stress calculation: This material features an additive split of matrix and reinforcement contributions, i.e. the combined stress response 𝝈 equals the sum 𝝈𝑚 + 𝝈𝑓 . The matrix mechanics is described by an elasto-plastic material formulation with a von-Mises yield criterion. The contribution of the reinforcement is formulated as a hyperelastic material. Based 0 is on the orientation angel 𝛼𝑖 of the i-th fiber family an initial fiber direction 𝐦𝑖 computed. By using the deformation gradient 𝐅 the current fiber configuration is 0 containing all necessary information on fiber strain and defined as 𝐦i = 𝐅 𝐦𝑖 reorientation. Following standard textbook mechanics for anisotropic and hyperelastic materials, the elastic stresses within the fibers due to tension or compression are given as 𝑓 = ∑ 𝑖=1 where the function 𝑓𝑖 of the fiber stretch 𝜆𝑖 corresponds to the load curve LCEFi. , 𝑓𝑖(𝜆𝑖)(𝐦i ⊗ 𝐦i) 𝝈𝑇 The shear behavior of the reinforcement can be controlled by METHij. For values less than 10, the behavior is again standard textbook mechanics: 𝝈𝑆 𝑓 = ∑ 𝑖=1 𝑔𝑖,𝑖+1(𝜅𝑖,𝑖+1)(𝐦i ⊗ 𝐦i+1) Where 𝜅𝑖,𝑖+1 represents the employed shear measure (scalar product or shear angle in rad). In general, the dyadic product 𝐦i ⊗ 𝐦i+1 does not define a shear stress tensor. This might result in unphysical shear behavior in case of woven fabrics. Therefore, 𝑓 is always METHij = 10 or 11 have been devised such that a pure shear stress tensor 𝝈𝑆 obtained. For even values of METHij, an elastic shear response is assumed. If defined, the load curve LCGij corresponds to function 𝑔𝑖,𝑗. In this case the values of Gij, ALOCij and GLOCij are ignored. For odd values of METHij on the other hand, an elasto-plastic shear behavior is assumed and the load curve LCGij defines the yield stress value as function of a normalized shear parameter. This implies that the load curve has to be defined for abscissa values between 0.0 and 1.0. A first elastic regime, which is controlled by the linear shear stiffness Gij, is assumed until the yield stress given in the load curve for normalized shear value 0.0 is reached. A second linear elastic regime is defined for shear angles (𝜉𝑖𝑗)/ fiber angles (𝜂𝑖𝑗) larger than the locking angle ALOCij. The corresponding stiffness in that regime is GLOCij. At the transition point to the second elastic regime, the shear stress corresponds to the load curve value for a normalized shear of 1.0. History data: This material formulation outputs additional data for post-processing to the set of history variables if requested by the user. The parameter POSTV defines the data to be written. Its value is calculated as POSTV = a1 + 2 𝑎2 + 4 𝑎3 + 8 𝑎4 + 16 𝑎5 + 32 𝑎6. Each flag 𝑎𝑖 is a binary (can be either 1 or 0) and corresponds to one particular post- processing variable according to the following table. Flag Description Variables # hist 𝑎1 𝑎2 𝑎3 𝑎4 𝑎5 𝑎6 Fiber angle Fiber ID Fiber stretch Fiber direction 𝜂12, 𝜂23 IDF1, IDF2, IDF3 𝜆1, 𝜆2, 𝜆3 𝐦1, 𝐦2, 𝐦3 Individual fiber stresses 𝑓1(𝜆1), 𝑓2(𝜆2), 𝑓3(𝜆3) Fiber stress tensor , 𝜎22 , 𝜎33 , 𝜎12 , 𝜎23 , 𝜎11 𝜎31 2 3 3 9 3 6 The above table also shows the order of output as well as the number of extra history variables associated with the particular flag. In total NXH extra variables are required depending on the choice of parameter POSTV. For example, the maximum number of additional variables is NXH = 26 for POSTV = 63. The post-processing data are written prior to most of the algorithmic history variables. A list of potentially helpful history variables are given in the following table. Position Description 3 Number of Fibers 4 NXH 5→NXH+4 Extra post-processing output NXH+5, NXH+6 Shear angles 𝜉12and 𝜉23 NXH+7 → NXH+12 Matrix stress tensor NXH+13 → NXH+21 Deformation gradient This is material type 249. It describes a material with unidirectional fiber reinforce- ments and considers up to three distinguished fiber directions. Each fiber family is described by a spatially transversely isotropic neo-Hookean constitutive law. The implementation is based on an adapted version of the material described by Bonet and Burton (1998). The material is only available for thin shell elements and in explicit simulations. Card 1 1 Variable MID Type A8 Card 2 1 2 RO F 2 Variable NFIB AOPT Type I F Card 3 Variable 1 V1 Type F Card 4 1 2 V2 F 2 3 EM 4 PRM F F 3 XP F 3 V3 F 3 4 YP F 4 D1 F 4 Variable IDF1 ALPH1 EF1 KAP1 Type I F F F 5 G F 5 ZP F 5 D2 F 5 6 7 8 EZDEF F 6 A1 F 6 7 A2 F 7 D3 MANGL F 6 F 7 8 A3 F 8 *MAT_249_UDFIBER *MAT_REINFORCED_THERMOPLASTIC_UDFIBER Card 5 1 2 3 4 5 6 7 8 Variable IDF2 ALPH2 EF2 KAP2 Type I F F F Card 6 1 2 3 4 5 6 7 8 Variable IDF3 ALPH3 EF3 KAP3 Type I F F F VARIABLE DESCRIPTION MID RO EM PR G Material identification. A unique number or label not exceeding 8 characters must be specified. Density. Isotropic young’s modulus 𝐸iso. Poisson’s ratio 𝑣. Linear shear modulus 𝐺fib. EZDEF Algorithmic parameter. If set to 1, last row of deformation gradient is not updated during the calculation. NFIB Number of fiber families to be considered. *MAT_REINFORCED_THERMOPLASTIC_UDFIBER *MAT_249_UDFIBER VARIABLE AOPT DESCRIPTION Material axes option : EQ.0.0: locally orthotropic with material axes determined by element with nodes, *DEFINE_COORDINATE_NODES, and then rotated about the shell element normal by the angle MANGL. as EQ.2.0: globally orthotropic with material axes determined by with below, vectors defined *DEFINE_COORDINATE_VECTOR. as EQ.3.0:: locally orthotropic material axes determined by rotating the material axes about the element normal by an angle, MANGL, from a line in the plane of the ele- ment defined by the cross product of the vector v with the element normal LT.0.0: the absolute value of AOPT is a coordinate system ID number (CID on *DEFINE_COORDINATE_NODES, *DEFINE_COORDINATE_SYSTEM or *DEFINE_COORDINATE_VECTOR). XP, YP, ZP Coordinates of point p for AOPT = 1. A1, A2, A3 Components of vector a for AOPT = 2. V1, V2, V3 Components of vector v for AOPT = 3. D1, D2, D3 Components of vector d for AOPT = 2. MANGL Material angle in degrees for AOPT = 0 and 3, may be overwritten on the element card, see *ELEMENT_SHELL_BETA. IDFi ID for i-th fiber family for post-processing. ALPHi EFi KAPi Orientation angle 𝛼𝑖 for i-th fiber with respect to overall material direction Young’s modulus 𝐸𝑖 for i-th fiber family. Fiber volume ratio 𝜅𝑖 of i-th fiber family. *MAT_249_UDFIBER *MAT_REINFORCED_THERMOPLASTIC_UDFIBER Stress calculation: In this model up to three distinguished fiber families are considered. It is assumed that there is no interaction between the families and, thus, that the resulting stress tensor is given by the sum of the single fiber responses, each to be calculated as the sum of an iso isotropic and a spatially transversely isotropic neo-Hookean stress contribution, 𝝈𝑖 tr , respectively. The implementation is based on the work of Bonet and Burton and 𝝈𝑖 (1998), adapted by BMW for simulation of unidirectional fabrics, see references below. In order to determine the isotropic stress tensor 𝝈𝑖 an isotropic bulk modulus 𝜆𝑖 have to be defined from the input values as: 𝑖𝑠𝑜, an isotropic shear modulus 𝜇 and 𝜇 = 𝐸iso 2(1 + 𝜈) and 𝜆𝑖 = 𝐸iso(𝜈 + 𝑛𝑖𝜈2) . 2(1 + 𝜈) Here, the variable 𝑛𝑖 denotes the ratio between stiffness orthogonally to the fibers and in fiber direction, i.e. 𝑛𝑖 = 𝐸iso/𝐸𝑖. Using the left Cauchy-Green tensor 𝒃 the isotropic neo- Hookean model reads: iso = 𝝈𝑖 (𝒃 − 𝑰) + 𝜆𝑖(𝐽 − 1)𝑰. 0 is Based on the orientation angel 𝛼𝑖 of the i-th fiber family an initial fiber direction 𝐦𝑖 computed. The deformation gradient 𝐅 is used to define the current fiber configuration 0. This vector contains all necessary information on fiber elongation and as 𝐦i = 𝐅 𝐦𝑖 reorientation. The spatially transversely isotropic neo-Hookean formulation is given by: 𝐽𝝈𝑖 tr = 2𝛽𝑖(𝐼4 − 1)𝑰 + 2(𝛼 + 2𝛽𝑖ln𝐽 + 2𝛾𝑖(𝐼4 − 1))𝐦i ⊗ 𝐦i − 𝛼(𝒃𝐦i ⊗ 𝐦i + 𝐦i ⊗ 𝒃𝐦i) with material parameters 𝛼 = 𝜇 − 𝐺fib, 𝛽𝑖 = 𝐸iso𝜈2(1 − 𝑛𝑖) 4𝑚𝑖(1 + 𝜈) , 𝑚𝑖 = 1 − 𝜈 − 2𝑛𝑖𝜈2, 𝛾𝑖 = 𝐸𝑖 𝜅𝑖(1 − 𝜈) 8𝑚 − 𝜆𝑖 + 2𝜇 + − 𝛽𝑖. The parameter EZDEF activates a modification of the model. Instead of the standard deformation gradient 𝐅, a modified tensor 𝐅̃ is employed to calculate current fiber directions 𝐦i and left Cauchy-Green tensor 𝒃. In tensor 𝐅̃ only the first two rows of the deformation gradient are updated based on the deformation of the element. This *MAT_REINFORCED_THERMOPLASTIC_UDFIBER *MAT_249_UDFIBER simplification can in some cases increase the stability of the model especially if the structure undergoes large deformations. References: -Bonet, J., and A. J. Burton. "A simple orthotropic, transversely isotropic hyperelas- tic constitutive equation for large strain computations." Computer methods in applied mechanics and engineering 162.1 (1998): 151-164. -Senner, T., et al. "A modular modeling approach for describing the in-plane forming behavior of unidirectional non-crimp-fabrics." Production Engineering 8.5 (2014): 635-643. -Senner, T., et al. "Bending of unidirectional non-crimp-fabrics: experimental characterization, constitutive modeling and application in finite element simula- tion." Production Engineering 9.1 (2015): 1-10. History data: Position Description 3 4 5 ID of 1st fiber ID of 2nd fiber ID of 3rd fiber 6 → 8 Current direction of 1st fiber 9 → 11 Current direction of 2nd fiber 12 → 14 Current direction of 3rd fiber 15 Number of fibers 16 Projected orthogonal fiber strain (1st fiber) 17 Projected parallel fiber strain (1st fiber) 18 Shear angle (1st fiber) in rad 19 Euler-Almansi strain (1st fiber) 20 Porosity (1st fiber) 21 Fiber volume ratio (1st fiber) 22 Projected orthogonal fiber strain (2nd fiber) 23 Projected parallel fiber strain (2nd fiber) 24 Shear angle (2nd fiber) in rad 25 Euler-Almansi strain (2nd fiber) *MAT_249_UDFIBER *MAT_REINFORCED_THERMOPLASTIC_UDFIBER 26 Porosity (2nd fiber) 27 Fiber volume ratio (2nd fiber) 28 Projected orthogonal fiber strain (3rd fiber) 29 Projected parallel fiber strain (3rd fiber) 30 Shear angle (3rd fiber) in rad 31 Euler-Almansi strain (3rd fiber) 32 Porosity (3rd fiber) 33 Fiber volume ratio (3rd fiber) *MAT_251 This is Material Type 251. It is similar to MAT_PIECEWISE_LINEAR_PLASTICITY or MAT_024 , except for the 3-D table option that uses a history variable (e.g. hardness, temperature, …) from a previous calculation to evaluate the plastic behavior as a function of 1) history variable, 2) strain rate, and 3) plastic strain. Only available for shell elements. Card 1 1 Variable MID 2 RO Type A8 F 3 E F 4 PR F 5 6 7 8 FAIL TDEL F Default none none none none 10.E+20 Card 2 1 2 3 4 Variable Type Default Card 3 1 2 LCSS F 0 3 4 5 VP F 0 5 6 7 HISVN PHASE I 0 6 F 0 7 F 0 8 8 Variable EPS1 EPS2 EPS3 EPS4 EPS5 EPS6 EPS7 EPS8 Type Default F 0 F 0 F 0 F 0 F 0 F 0 F 0 F Card 4 1 2 3 4 5 6 7 8 Variable ES1 ES2 ES3 ES4 ES5 ES6 ES7 ES8 Type Default F 0 F 0 F 0 F 0 F 0 F 0 F 0 F 0 VARIABLE DESCRIPTION MID RO E PR Material identification. A unique number or label not exceeding 8 characters must be specified. Mass density. Young’s modulus. Poisson’s ratio. FAIL Failure flag. LT.0.0: User defined failure subroutine, matusr_24 in dyn21.F, is called to determine failure EQ.0.0: Failure is not considered. This option is recommended if failure is not of interest since many calculations will be saved. GT.0.0: Effective plastic strain to failure. When the plastic strain reaches this value, the element is deleted from the calculation. TDEL LCSS Minimum time step size for automatic element deletion. Load curve ID or Table ID . Load curve for stress vs. plastic strain. 2-D table for stress vs. plastic strain as a function of strain rates. 3-D table for stress vs. plastic strain as a function of strain rates as a function of history variable values . VP Formulation for rate effects: EQ.0.0: Scale yield stress (default), EQ.1.0: Viscoplastic formulation. HISVN Location of history variable in the history array of *INITIAL_- STRESS_SHELL that is used to evaluate the 3-D table LCSS. VARIABLE PHASE EPS1 - EPS8 DESCRIPTION Constant value to evaluate the 3-D table LCSS. Only used if HISVN = 0. Effective plastic strain values (optional). At least 2 points should be defined. The first point must be zero corresponding to the initial yield stress. ES1 - ES8 Corresponding yield stress values to EPS1 - EPS8. Remarks: If the 3-D table is used for LCSS, interpolation is used to find the corresponding stress value for the current plastic strain, strain rate, and history variable. In addition, extrapolation is used for the history variable evaluation, which means that some upper and lower “limit curves” have to be used, if extrapolation is not desired. If material history is written to dynain file using *INTERFACE_SPRINGBACK_LS- DYNA, the history variable of material 251 (e.g. hardness, temperature, …) is written to position HISV6 of *INITIAL_STRESS_SHELL. It is recommended to set HISVN = 6 and to put the history variable on position HISV6 if *MAT_251 is used in combination with *MAT_ADD_... *MAT_TOUGHENED_ADHESIVE_POLYMER This is Material Type 252, the Toughened Adhesive Polymer model (TAPO). It is based on non-associated 𝐼1 - 𝐽2 plasticity constitutive equations and was specifically developed to represent the mechanical behaviour of crash optimized high-strength adhesives under combined shear and tensile loading. This model includes material softening due to damage, rate-dependency, and a constitutive description for the mechanical behaviour of bonded connections under compression. A detailed description of this material can be found in Matzenmiller and Burbulla [2013]. This material model can be used with solid elements or with cohesive elements in combination with *MAT_ADD_COHESIVE. Card 1 1 Variable MID Type A8 Card 2 1 2 RO F 2 Variable LCSS TAU0 Type I Card 3 1 F 2 3 E F 3 Q F 3 4 PR F 4 B F 4 5 6 7 8 FLG JCFL DOPT I 5 H F 5 I 6 C F 6 I 7 8 GAM0 GAMM F 7 F 8 Variable A10 A20 A1H A2H A2S POW Type F Card 4 1 F 2 Variable Type F F F F 3 D1 F 4 D2 F 5 D3 F 6 D4 F 7 8 D1C D2C F VARIABLE DESCRIPTION MID RO E PR FLG Material identification. A unique number or label not exceeding 8 characters must be specified. Mass density 𝜌. Young’s modulus 𝐸. Poisson’s ratio 𝜈. Flag to choose between yield functions 𝑓 and 𝑓 ̂, see Remarks. EQ.0.0: Cap in tension. and Drucker & Prager in compression, EQ.2.0: Cap in tension. and von Mises in compression. JCFL Johnson & Cook constitutive failure criterion flag, see Remarks. EQ.0.0: use triaxiality factor only in tension, EQ.1.0: use triaxiality factor in tension and compression. DOPT Damage criterion flag 𝐷̂ or 𝐷̌ , see Remarks. EQ.0.0: damage model uses damage plastic strain 𝑟, EQ.1.0: damage model uses plastic arc length 𝛾v. LCSS Curve ID or Table ID. If LCSS is a curve ID: The curve specifies yield stress 𝜏Y as a function of plastic strain 𝑟. If LCSS is a Table ID: For each strain rate value the table specifies a curve ID giving the yield stress versus plastic strain for that strain rate or it defines for each tempera- ture value a table ID which, in turn, maps strain rates to curves giving the yield stress as a function of plastic strain . The yield stress versus plastic strain curve for the lowest value of strain rate or temperature is used when the strain rate or temperature falls below the minimum value. Likewise, maximum values cannot be exceeded. Harden- ing variables are ignored with this option (TAU0, Q, B, H, C, GAM0, and GAMM). *MAT_TOUGHENED_ADHESIVE_POLYMER DESCRIPTION TAU0 Initial shear yield stress 𝜏0. Q B H C Isotropic nonlinear hardening modulus 𝑞. Isotropic exponential decay parameter 𝑏. Isotropic linear hardening modulus 𝐻. Strain rate coefficient 𝐶. GAM0 GAMM Quasi-static threshold strain rate 𝛾0. Maximum threshold strain rate 𝛾m. Yield function parameter: initial value 𝑎10 of 𝑎1 = 𝑎 ̂1(𝑟). Yield function parameter: initial value 𝑎20 of 𝑎2 = 𝑎 ̂2(𝑟). Yield function parameter 𝑎1 (ignored if FLG.EQ.2). H for formative hardening Yield function parameter 𝑎2 (ignored if FLG.EQ.2). H for formative hardening Plastic potential parameter 𝑎2 ∗ for hydrostatic stress term. Exponent 𝑛 of the phenomenological damage model. Johnson & Cook failure parameter 𝑑1. Johnson & Cook failure parameter 𝑑2. Johnson & Cook failure parameter 𝑑3. Johnson & Cook rate dependent failure parameter 𝑑4. Johnson & Cook damage threshold parameter 𝑑1c. Johnson & Cook damage threshold parameter 𝑑2c. A10 A20 A1H A2H A2S POW D1 D2 D3 D4 D1C D2C Remarks: Two different 𝐼1-𝐽2 yield criteria for isotropic plasticity can be defined by parameter FLG: Figure M252-1. Yield function 𝑓 and plastic flow potential 𝑓 ∗ Figure M252-2. Yield function 𝑓 ̂ and plastic flow potential 𝑓 ∗ 1. FLG = 0 is used for the yield criterion 𝑓 which is changed at the case of hydrostatic pressure 𝐼1 = 0 into the Drucker & Prager model (DP) 𝑓 ≔ 𝐽2 (1 − 𝐷)2 + √3 𝑎1𝜏0 𝐼1 1 − 𝐷 + 𝑎2 ⟨ 𝐼1 1 − 𝐷 ⟩ − 𝜏Y 2 = 0 with the Macauley bracket 〈∙〉, the first invariant of the stress tensor 𝐼1 = tr 𝛔, and the second invariant of the stress deviator 𝐽2 = (1 2⁄ )tr(𝐬)2, see Figure M252-1. 2. FLG = 2 is used for the yield criterion 𝑓 ̂ which is changed at the vertex into the deviatoric von Mises yield function – see Figure M252-2 – and is used for con- servative calculation in case of missing uniaxial compression or combined com- pression and shear experiments: 𝑓 ̂ ≔ 𝐽2 (1 − 𝐷)2 + 𝑎2 ⟨ 𝐼1 1 − 𝐷 + √3𝑎1𝜏0 2𝑎2 ⟩ − (𝜏Y 2 + 2𝜏0 𝑎1 4𝑎2 ) = 0 The yield functions 𝑓 and 𝑓 ̂ are formulated in terms of the effective stress tensor and the isotropic material damage 𝐷 according to the continuum ⁄ 𝛔̃ = 𝛔 (1 − 𝐷) Figure M252-3. Accumulated plastic strain 𝛾v and damage plastic strain 𝑟 versus strain 𝛾 damage mechanics in Lemaitre [1992]. The stress tensor 𝛔 is defined in terms of the elastic strain 𝛆e and the isotropic damage 𝐷: 𝛔 = (1 − 𝐷)ℂ𝛆e The continuity (1 − 𝐷) in the elastic constitutive equation above degrades the fourth order elastic stiffness tensor ℂ, ℂ = 2𝐺 (𝕀 − 𝟏⨂𝟏) + 𝐾 𝟏⨂𝟏 with shear modulus 𝐺, bulk modulus 𝐾, fourth order identity tensor 𝕀, and second order identity tensor 𝟏. The plastic strain rate 𝛆̇p is given by the non-associated flow rule (1 − 𝐷)2 (𝐬 + with the potential 𝑓 ∗ and an additional parameter 𝑎2 = 𝛆̇p = 𝜆 𝜕𝑓 ∗ 𝜕𝛔 ∗〈𝐼1〉𝟏) 𝑎2 ∗ < 𝑎2 to reduce plastic dilatancy. 𝑓 ∗ ≔ 𝐽2 (1 − 𝐷)2 + ∗ 𝑎2 ⟨ 𝐼1 1 − 𝐷 ⟩ 2 − 𝜏Y The plastic arc length 𝛾̇v characterizes the inelastic response of the material and is defined by the Euclidean norm: 𝛾̇v ≔ √2 tr(𝛆̇p)2 = 2𝜆 (1 − 𝐷)2 √𝐽2 + (𝑎2 ∗〈𝐼1〉)2 In addition, the arc length of the damage plastic strain rate 𝑟 ̇ is introduced by means of the arc length 𝛾̇v and the continuity (1 − 𝐷) as in Lemaitre [1992], where 𝐼 ̃1 = 𝐼1 (1 − 𝐷) and 𝐽 ̃2 = 𝐽2 (1 − 𝐷)2 ⁄ are the effective stress invariants, see Figure M252-3. ⁄ 𝑟 ̇ ≔ (1 − D)𝛾̇v = 2λ√𝐽 ̃2 + ∗⟨𝐼 ̃1⟩) (𝑎2 The rate-dependent yield strength for shear 𝜏Y can be defined by two alternative expressions. The first representation is an analytic expression for 𝜏Y: 𝜏Y = (𝜏0 + 𝑅) [1 + 𝐶 (⟨ln 𝛾̇ 𝛾̇0 ⟩ − ⟨ln 𝛾̇ 𝛾̇m ⟩)] , with 𝛾̇ = √2 tr(𝛆̇)2 where the first factor (𝜏0 + 𝑅) in 𝜏Y is given by the static yield strength with the initial yield 𝜏0 and the non-linear hardening contribution 𝑅 = 𝑞[1 − exp(−𝑏𝑟)] + 𝐻𝑟 The second factor [… ] in 𝜏Y describes the rate dependency of the yield strength by a modified Johnson & Cook approach with the reference strain rates 𝛾̇0 and 𝛾̇m which Figure M252-4. Rate-dependent tensile strength 𝜏Y versus effective strain rate 𝛾̇ (left) and effective damage plastic strain 𝑟 (right) limit the shear strength 𝜏Y, see Figure M252-4. The second representation of the yield strength 𝜏Y is the table definition LCSS, where hardening can be defined as a function of plastic strain, strain rate, and temperature. Toughened structural adhesives show distortional hardening under plastic flow, i.e. the yield surface changes its shape. This formative hardening can be phenomenological described by simple evolution equations of parameters 𝑎1 = 𝑎 ̂1(𝑟) ∧ 𝑎2 = 𝑎 ̂2(𝑟) in the yield criterions 𝑓 with the initial values 𝑎10 and 𝑎20: H𝑟 ̇ 𝑎1 = 𝑎 ̂1(𝑟) ∧ 𝑎 ̇1 = 𝑎1 𝑎2 = 𝑎 ̂2(𝑟) ∧ 𝑎2 ≥ 0 ∧ 𝑎 ̇2 = 𝑎2 H𝑟 ̇ H and 𝑎2 H can take positive or negative values as long as the inequality The parameters 𝑎1 𝑎2 ≥ 0 is satisfied. The criterion 𝑎2 ≥ 0 ensures an elliptic yield surface. The yield criterion 𝑓 ̂ uses only the initial values 𝑎1 = 𝑎10 and 𝑎2 = 𝑎20 without the distortional hardening. The empirical isotropic damage model 𝐷 is based on the approach in Lemaitre [1985]. Two different evolution equations 𝐷̂̇ (𝑟, 𝑟 ̇) and 𝐷̌̇ (𝛾v, 𝛾̇v) are available, Figure M252-5 see. The damage variable 𝐷 is formulated in terms of the damage plastic strain rate 𝑟 ̇ (DOPT = 0) 𝐷̇ = 𝐷̂̇ (𝑟, 𝑟 ̇) = 𝑛 ⟨ 𝑛−1 𝑟 − 𝛾c 𝛾f − 𝛾c ⟩ 𝑟 ̇ 𝛾f − 𝛾c Figure M252-5. Influence of DOPT on damage softening or of the plastic arc length 𝛾̇v (DOPT = 1) 𝐷̇ = 𝐷̌̇ (𝛾v, 𝛾̇v) = 𝑛 ⟨ 𝑛−1 𝛾v − 𝛾c 𝛾f − 𝛾c ⟩ 𝛾̇v 𝛾f − 𝛾c where r in contrast to 𝛾v increases non-proportionally slowly, see Figure M252-5. The strains at the thresholds 𝛾c and 𝛾f for damage initiation and rupture are functions of the triaxiality 𝑇 = 𝜎m 𝜎eq⁄ with the hydrostatic stress 𝜎m = 𝐼1 3⁄ and the von Mises equivalent stress 𝜎eq = √3𝐽2 as in Johnson and Cook [1985]. 𝛾c = [𝑑1c + 𝑑2cexp(−𝑑3〈𝑇〉)] (1 + 𝑑4 ⟨ln ⟩) 𝛾f = [𝑑1 + 𝑑2exp(−𝑑3〈𝑇〉)] (1 + 𝑑4 ⟨ln ⟩) 𝛾̇ 𝛾̇0 𝛾̇ 𝛾̇0 The option JCFL controls the influence of triaxiality 𝑇 = 𝜎m 𝜎eq⁄ in the pressure range for the thresholds 𝛾c and 𝛾f. JCFL = 0 makes use of the Macauley bracket 〈𝑇〉 for the triaxiality 𝑇 = 𝜎m 𝜎eq⁄ and JCFL = 1 omits the Macauley bracket 〈𝑇〉. History Variables: VARIABLE DESCRIPTION 1 2 3 4 5 6 7 damage variable 𝐷 plastic arc length 𝛾v effective strain rate temperature yield stress damaged yield stress triaxiality *MAT_GENERALIZED_PHASE_CHANGE This is Material Type 254. It is designed to model phase transformations in metallic materials and the implied changes in the material properties. It is applicable to hot stamping, heat treatment and welding processes and a wide range of steel alloys. It accounts for up to 24 phases and provides a list of generic phase change mechanisms for each possible phase changes. The parameters for the phase transformation laws are to be given in tabulated form. Given the current microstructure composition, the material formulation implements a temperature and strain-rate dependent elastic-plastic material with non-linear hardening behavior. Above a certain annealing temperature, the material behaves as ideal elastic-plastic material with no evolution of plastic strains. So far, the material has been implemented for solid and shell elements and is suitable for explicit and implicit analysis. Card 1 1 Variable MID Type A8 Card 2 1 2 RO F 2 3 N I 3 4 YM F 4 5 PR F 5 6 7 8 MIX MIXR I 6 I 7 8 Variable TASTRT TAEND CTE DTEMP TIME Type F Card 3 1 F 2 I 3 4 5 6 F 7 F 8 Variable PTLAW PTSTR PTEND PTX1 PTX2 PTX3 PTX4 PTX5 Type I I I I I I I Card 4 1 2 3 4 5 6 7 8 Variable PTTAB1 PTTAB2 PTTAB3 PTTAB4 PTTAB5 Type Card 5 I 1 I 2 I 3 I 4 I 5 6 7 8 Variable PTEPS PTRIP Type I F GRAI F Phase Yield Stress Cards. For each of the N phases, one parameter SIGYi has to be specified. A keyword card (with a “*” in column 1) terminates this input if less than 10 cards are used. Optional 1 2 3 4 5 6 7 8 Variable SIGY1 SIGY2 SIGY3 SIGY4 SIGY5 SIGY6 SIGY7 SIGY8 Type I I I I I I I I VARIABLE DESCRIPTION MID RO N YM Material identification. A unique number or label not exceeding 8 characters must be specified. Mass density 𝜌. Number of phases Youngs’ modulus: GT.0.0: constant value is used LT.0.0: LCID or TABID. Temperature dependent Youngs’ modulus given by load curve ID = -E or a Table ID = -E. Use TABID to describe temperature de- pendent modulus for each phase individually. VARIABLE DESCRIPTION PR Poisson’s modulus: GT.0.0: constant value is used LT.0.0: LCID or TABID. Temperature dependent Posson’s ratio given by load curve ID = -E or a Ta- ble ID = -E. Use TABID to describe temperature dependent parameter for each phase individually. MIX MIXR Load curve ID with initial phase concentrations LCID or TABID for mixture rule. Use a TABID to define a temperature dependency TASTART TAEND Annealing temperature start Annealing temperature end CTE Coefficient of thermal expansion: GT.0.0: constant value is used LT.0.0: LCID or TABID. Temperature dependent CTE given by load curve ID = -CTE or a Table ID = - CTE. Use Table ID to describe temperature de- pendent CTE for each phase individually. DTEMP TIME Maximum temperature variation within a time step. If exceeded during the analysis a local sub-cycling is used Number of time units per hour. Default is seconds, that is 3600 time units per hour. PTLAW PTSTR PTEND PTXi *MAT_GENERALIZED_PHASE_CHANGE DESCRIPTION Table ID to define phase transformation model as a function of source phase and target phase. The values in *DEFINE_TABLE are the phase numbers before transformation (source phase). The curves referenced by the table specify transformation model (ordinate) versus phase number after transformation (abscissa). LT.0: Transformation model used in cooling EQ.0: No transformation GT.0: Transformation model is used in heating There are four possible transformation models which can be specified as ordinate values of the curves: EQ.1: Koinstinen-Marburger EQ.2: JMAK EQ.3: Akerstrom (only for cooling) EQ.4: Oddy (only for heating) Table ID to define start temperatures for the transformations as function of source phase and target phase. The values in *DEFINE_TABLE are the phase numbers before transformation (source phase). The curves referenced by the table specify start temperature (ordinate) versus phase number after transformation (abscissa). Table ID to define end temperatures for the transformations as function of source phase and target phase. The values in *DEFINE_TABLE are the phase numbers before transformation (source phase). The curves referenced by the table specify end temperature (ordinate) versus phase number after transformation (abscissa). Table ID defining the i-th scalar-valued phase transformation parameter as function of source phase and target phase . The values in *DEFINE_TABLE are the phase numbers before transformation (source phase). The curves referenced by the table specify scalar parameter (ordinate) versus phase number after transformation (abscissa). VARIABLE PTTABi PTEPS PTRIP DESCRIPTION i-th tabulated phase Table ID of 3D table defining the transformation parameter as function of source phase and target phase . The values in *DEFINE_TABLE_3D are the phase numbers before transformation (source phase). The values in the 2D tables referenced by *DEFINE_TABLE_3D are the phase number after transformation. The curves referenced by the 2D tables specify tabulated parameter (ordinate) versus either temperature or temperature rate (abscissa). Table ID containing transformation induced strains as function of source phase and target phase. Flag for transformation induced plasticity (TRIP). Algorithm active for positive value of PTRIP. GRAIN Initial grain size. Remarks: This material features temperature and phase composition dependent elastic plastic behavior. The phase composition is determined using a list of generic phase transformation mechanisms the user can choose from for each of the possible phase transformations. So far, four different transformation models have been implemented to describe the transition from source phase 𝑥a to target phase 𝑥b: 1. Koistinen-Marburger: This formulation is tailored for non-diffusive transformations. The tempera- ture dependent amount of the target phase is computed as The factor 𝛼 is to be defined in table PTX1. 𝑥𝑏 = 𝑥𝑎(1.0 − 𝑒−𝛼(𝑇𝑠𝑡𝑎𝑟𝑡−𝑇)) 2. Generalized Johnson-Mehl-Avrami-Kolmogorov (JMAK): This widely used model employs the evolution equation 𝑑𝑥𝑏 𝑑𝑡 = 𝑛(𝑇)(𝑘𝑎𝑏𝑥𝑎 − 𝑘𝑎𝑏 ′ 𝑥𝑏) for which the factors ⎜⎛ln ( ⎝ 𝑘𝑎𝑏(𝑥𝑎 + 𝑥𝑏) ′ 𝑥𝑏 𝑘𝑎𝑏𝑥𝑎 − 𝑘𝑎𝑏 ) ⎟⎞ ⎠ 𝑛(𝑇)−1.0 𝑛(𝑇) 𝑘𝑎𝑏 = 𝑥𝑒𝑞(𝑇) 𝜏(𝑇) 𝑓 (𝑇̇), 𝑘𝑎𝑏 ′ = 1.0 − 𝑥𝑒𝑞(𝑇) 𝜏(𝑇) 𝑓 ′(𝑇̇) have to be defined. As user input, load curve data for the exponent 𝑛(𝑇) in PTTAB1, the equilibri- um concentration 𝑥𝑒𝑞(𝑇) in PTTAB2, the relaxation time 𝜏(𝑇) in PTTAB3, and the temperature rate correction factors 𝑓 (𝑇̇) and 𝑓′(𝑇̇) in PTTAB4 and PTTAB5, respectively, are expected. 3. Kirkaldy: Similar to the implementation of *MAT_244, the transformation for cooling phases can be computed by the evolution equation 𝑑𝑋𝑏 𝑑𝑡 = 20.5(𝐺−1)𝑓 (𝐶)(𝑇𝑠𝑡𝑎𝑟𝑡 − 𝑇)𝑛𝑇𝐷(𝑇) 𝑋𝑏 𝑛1(1.0−𝑋𝑏)(1.0 − 𝑋𝑏)𝑛2𝑋𝑏 Y(𝑋𝑏) 𝑥𝑏 . 𝑥𝑒𝑞(𝑇) formulated in the normalized phase concentration 𝑋𝑏 = In contrast to *MAT_244, the parameters for the evolution equation are not determined from the chemical composition of the material but defined directly as user input. The scalar data in PTX1 to PTX4 are interpreted as 𝑓 (𝐶), 𝑛𝑇, 𝑛1, and 𝑛2. Tabulated data for 𝐷(𝑇), 𝑌(𝑋𝑏), and 𝑥𝑒𝑞(𝑇) are given in PTTAB1 to PTTAB3. 4. Oddy: For phase transformation in heating, the equation of Oddy can be used, which can be interpreted as a simplified JAMK relation and reads 𝑑𝑥𝑏 𝑑𝑡 = 𝑛 𝑥𝑎 𝑐1(𝑇 − 𝑇𝑠𝑡𝑎𝑟𝑡)−𝑐2 ⎝ ⎜⎛ln ( (𝑥𝑎 + 𝑥𝑏) 𝑥𝑎 ⎟⎞ ) ⎠ 𝑛−1.0 Its application requires the input of three scalar parameters 𝑛, 𝑐1, 𝑐2 that are read from the respective positions in the tables in PTX1 to PTX3. *MAT_PIECEWISE_LINEAR_PLASTIC_THERMAL This is material type 255, an isotropic elastoplastic material with thermal properties. It can be used for both explicit and implicit analyses. Young’s modulus and Poisson’s ratio can depend on the temperature by defining two load curves. Moreover, the yield stress in tension and compression are given as load curves for different temperatures by using two tables. The thermal coefficient of expansion can be given as a constant ALPHA or as a load curve, see LALPHA at position 3 on card 2. A positive curve ID for LALPHA models the instantaneous thermal coefficient, whereas a negatives curve ID models the thermal coefficient relative to a reference temperature, TREF. The strain rate effects are modelled with the Cowper-Symonds rate model with the parameters C and P on card 1. Failure can be based on effective plastic strain or using the *MAT_ADD_- EROSION keyword. Card 1 1 Variable MID Type A8 Card 2 1 2 RO F 2 3 E F 3 Variable TABIDC TABIDT LALPHA Type I Card 3 1 I 2 I 3 Variable ALPHA TREF Type F F 4 PR F 4 4 5 C F 5 VP F 5 6 P F 6 7 8 FAIL TDEL F 7 F 8 6 7 8 VARIABLE MID DESCRIPTION Material identification. A unique number or label not exceeding 8 characters must be specified. RO Mass density. *MAT_PIECEWISE_LINEAR_PLASTIC_THERMAL DESCRIPTION E Young’s modulus: LT.0.0: E is given as a function of temperature, T. The curve consists of (T,E) data pairs. Enter |E| on the DE- FINE_CURVE keyword. GT.0.0: E is constant. PR Poisson’s ratio. LT.0.0: |PR| is the LCID for Poisson’s ratio versus tempera- C P FAIL TDEL ture. GT.0.0: PR is constant Strain rate parameter. See Remark 1. Strain rate parameter. See Remark 1. Effective plastic strain when the material fails. User defined failure subroutine, matusr_24 in dyn21.F, is called to determine failure when FAIL < 0. Note that for solids the *MAT_ADD_- EROSION can be used for additional failure criteria. A time step less than TDEL is not allowed. A step size less than TDEL trigger automatic element deletion. This option is ignored for implicit analyses. TABIDC Table ID for yield stress in compression, see Remark 2. TABIDT Table ID for yield stress in tension, see Remark 2. LALPHA Load curve ID for thermal expansion coefficient as a function of temperature. GT.0.0: the instantaneous thermal expansion coefficient based on the following formula: 𝑑𝜀𝑖𝑗 thermal = 𝛼(𝑇)𝑑𝑇𝛿𝑖𝑗 LT.0.0: the thermal coefficient is defined relative a reference temperature TREF, such that the total thermal strain is given by: thermal = 𝛼(𝑇)(𝑇 − 𝑇ref)𝛿𝑖𝑗 𝜀𝑖𝑗 With this option active, ALPHA is ignored. VARIABLE DESCRIPTION VP Formulation for rate effects, see Remarks 1 and 2. EQ.0.0: effective total strain rate (default) NE.0.0: effective plastic strain rate ALPHA Coefficient of thermal expansion TREF Reference temperature, which is required if and only if LALPHA is given with a negative load curve ID. Remarks: 1. Strain Rate Effects. The strain rate effect is modelled by using the Cowper and Symonds model which scales the yield stress according to the factor 1 + ( 𝜀̇eff 1 𝑃⁄ ) where 𝜀̇eff = √tr(𝛆̇𝛆̇T) is the Euclidean norm of the total strain rate tensor if 𝑝 . VP = 0 (default), otherwise 𝜀̇eff = 𝜀̇eff 2. Yield Stress Tables. The dependence of the yield stresses on the effective plastic strains is given in two tables. a) TABIDC gives the behaviour of the yield stresses in compression b) TABIDT gives the behaviour of the yield stresses in tension. The table indices consist of temperatures, and at each temperature a yield stress curve must be defined. Both TABIDC and TABIDT can be 3D tables, in which temperatures indexes the main table and strain rates are defined as values for the sub tables with harden- ing curves as targets for those strain rates. If the same yield stress should be used in both tension and compression, only one table needs to be defined and the same TABID is put in position 1 and 2 on card 2. If VP = 0, effective total strain rates are used in the 3D tables, otherwise plastic strain rates. 3. History Variables. Two history variables are added to the d3plot file, the Young’s modulus and the Poisson’s ratio, respectively. They can be requested through the *DATABASE_EXTENT_BINARY keyword. 4. Nodal Temperatures. Nodal temperatures must be defined by using a coupled analysis or some other way to define the temperatures, such as *LOAD_THERMAL_VARIABLE or *LOAD_THERMAL_LOAD_CURVE. *MAT_AMORPHOUS_SOLIDS_FINITE_STRAIN This is material type 256, an isotropic elastic-viscoplastic material model intended to describe the behaviour of amorphous solids such as polymeric glasses. The model accurately captures the hardening-softening-hardening sequence and the Bauschinger effect experimentally observed at tensile loading and unloading respectively. The formulation is based on hyperelasticity and uses the multiplicative split of the deformation gradient F which makes it naturally suitable for both large rotations and large strains. Stress computations are performed in an intermediate configuration and are therefore preceded by a pull-back and followed by a push-forward. The model was originally developed by Anand and Gurtin [2003] and implemented for solid elements by Bonnaud and Faleskog [2008] Card 1 1 Variable MID 2 RO Type A8 F Card 2 1 Variable ALPHA Type F 2 H0 F 3 K F 3 SCV F 4 G F 4 B F 5 MR F 5 ECV F 6 LL F 6 G0 F 7 NU0 F 7 S0 F 8 M F 8 VARIABLE DESCRIPTION MID RO K G MR LL NU0 Material identification. A unique number or label not exceeding 8 characters must be specified. Mass density Bulk modulus Shear modulus Kinematic hardening parameter: μR Kinematic hardening parameter: λL Creep parameter: ν0 *MAT_AMORPHOUS_SOLIDS_FINITE_STRAIN DESCRIPTION M ALPHA Creep parameter: m Creep parameter: α Isotropic hardening parameter: h0 Isotropic hardening parameter: scv Isotropic hardening parameter: b Isotropic hardening parameter: ηcv Isotropic hardening parameter: g0 Isotropic hardening parameter: s0 H0 SCV B ECV G0 S0 Remarks: 1. Kinematic hardening gives rise to the second hardening occurrence in the hardening-softening-hardening sequence. The constants μR and λL enter the back stress μB (where B is the left Cauchy-Green deformation tensor) through the function μ according to: 𝜇 = 𝜇𝑟 ( 𝜆𝐿 3𝜆𝑝) 𝐿−1 ( 𝜆𝑝 𝜆𝐿 ) (256.1) Where 𝜆𝑝 = 1 √3 √𝑡𝑟(𝐵𝑝) and 𝐵𝑝 is the plastic part of the left Cauchy-Green de- formation tensor and where L is the Langevin function defined by, 𝐿(𝑋) = coth(𝑋) − 𝑋−1 2. This material model assumes plastic incompressibility. Nevertheless in order to account for the different behaviours in tension and compression a Drucker- Prager law is included in the creep law according to: 𝜈𝑝 = 𝜈0 ( 𝜏̅ 𝑠 + 𝛼𝜋 𝑚⁄ ) (256.2) Where 𝜈𝑝 is the equivalent plastic shear strain rate, stress, s the internal variable defined below and -π the hydrostatic stress. the equivalent shear 3. Isotropic hardening gives rise to the first hardening occurrence in the harden- ing-softening-hardening sequence. Two coupled internal variables are defined: s the resistance to plastic flow and η the local free volume. Their evolution equations read: 𝑠 ̇ = ℎ0 [1 − 𝑠 ̃(𝜂) ] 𝜈𝑝 𝜂̇ = 𝑔0 ( 𝑠𝑐𝑣 − 1) 𝜈𝑝 𝑠 ̃(𝜂) = 𝑠𝑐𝑣[1 + 𝑏(𝜂𝑐𝑣 − 𝜂)] (256.3) (256.4) (256.5) 4. Typical material parameters values are given in Ref.1 for Polycarbonate: PolyC 1 1 Variable MID Value PolyC 2 1 Variable ALPHA 2 RO 2 H0 3 K 4 G 5 MR 6 LL 7 NU0 8 M 2.24GPa 0.857GPa 11.0MPa 1.45 0.0017s-1 0.011 3 SCV 4 B 5 ECV 6 G0 7 S0 8 Value 0.08 2.75GPa 24.0MPa 825 0.001 0.006 20.0MPa [1] Anand, L., Gurtin, M.E., 2003, “A theory of amorphous solids undergoing large deformations, with application to polymeric glasses,” International Journal of Solids and Structures, 40, pp. 1465-1487. *MAT_STOUGHTON_NON_ASSOCIATED_FLOW This is Material Type 260A. This material model is implemented based on non- associated flow rule models (Stoughton 2002 and 2004). Strain rate sensitivity can be included using a load curve. This model applies to both shell and solid elements. Available options include: <BLANK> XUE The option XUE is available for solid elements only. Card 1 1 2 Variable MID RO Type A8 F 3 E F 4 5 6 7 8 PR R00 R45 R90 SIG00 F F F F F Default none none none none none none none none Card 2 1 2 3 4 5 6 7 8 Variable SIG45 SIG90 SIG_B LCIDS LCIDV SCALE Type F F F I I F Default none none none none none 1.0 Define the following card only for the option XUE (available for solids only): 6 7 8 Card 3 1 2 Variable EF0 PLIM Type F F 3 Q F 4 GAMA F 5 M F Default none none none none none Card 3 1 2 3 4 5 6 7 8 Variable AOPT Type F Default none Card 4 1 Variable XP Type F 2 YP F 3 ZP F 4 A1 F 5 A2 F 6 A3 F 7 8 Default none none none none none none Card 5 1 Variable V1 Type F 2 V2 F 3 V3 F 4 5 6 7 8 D1 D2 D3 F F F Default none none none none none none VARIABLE DESCRIPTION MID RO E PR Material identification. A unique number or label not exceeding 8 characters must be specified. Mass density. Young’s Modulus Poisson’s ratio R00, R45, R90 Lankford parameters in rolling (0°), diagonal (45°) and transverse (90°) directions, respectively; determined from experiments. SIG00, SIG45, SIG90, SIG_B SIG00: the initial yield stress from uniaxial tension tests in rolling (0°) direction; SIG45: the initial yield stress from uniaxial tension tests in diagonal (45°) direction; SIG90: the initial yield stress from uniaxial tension tests in transverse (90°) directions; SIG_B: the initial yield stress from equi-biaxial stretching tests. LCIDS ID of a load curve defining stress vs. strain hardening behavior from a uniaxial tension test along the rolling direction. VARIABLE LCIDV SCALE DESCRIPTION ID of a load curve defining stress scale factors vs. strain rates; determined from experiments. An example of the curve can be found in Figure M260A-2. Furthermore, strain rates are stored in history variable #5. Strain rate scale factors are stored in history variable #6. To turn on the variables for viewing in LS-PrePost, set NEIPS to at least “6” in *DATABASE_EXTENT_BINARY. It is very useful to know what levels of strain rates, and strain rate scale factors in a particular simulation. Once d3plot files are opened in LS-PrePost, individual element time history can be plotted via menu option Post → History, or a color contour of the entire part can be viewed with the menu option Post → FriComp → Misc. This variable can be used to speed up the simulation while equalizing the strain rate effect, useful especially in cases where the pulling speed or punch speed is slow. For example, if the pulling speed is at 15 mm/s but running the simulation at this speed will take a long time, the pulling speed can be increased to 500 mm/s while "SCALE" can be set to 0.03, giving the same results as those from 15 mm/s, but with the benefit of greatly reduced computational time, see Figures M260A-3 and M260A-4. Note the increased absolute value (within a reasonable range) of mass scaling -1.0*dt2ms frequently used in forming simulation does not affect the strain rates, as shown in the Figure M260A-5. EF0, PLIM, Q, GAMA, M Material parameters for the option XUE. The parameter k in the original paper is assumed to be 1.0. For details, refer to Xue, L., Wierzbicki, T.’s 2009 paper “Numerical simulation of fracture mode transition in ductile plates” in the International Journal of Solids and Structures. AOPT *MAT_STOUGHTON_NON_ASSOCIATED_FLOW DESCRIPTION Material axes option : EQ.0.0: locally orthotropic with material axes determined by element nodes 1, 2, and 4, as with *DEFINE_COORDI- NATE_NODES, and then rotated about the shell ele- ment normal by the angle BETA. EQ.1.0: locally orthotropic with material axes determined by the point 𝐩 in space and the global location of the ele- ment center; this is the 𝐚-direction. This option is for solid elements only. EQ.2.0: globally orthotropic with material axes determined by the vector 𝐚 for shells and by both vectors 𝐚 and 𝐝 for solids, as with *DEFINE_COORDINATE_VECTOR. EQ.3.0: locally orthotropic material axes determined by rotating the material axes about the element normal by an angle, BETA, from a line in the plane of the element defined by the cross product of the vector 𝐯 with the element normal. The plane of a solid element is the mid-surface between the inner surface and outer sur- face defined by the first four nodes and the last four nodes of the connectivity of the element, respectively. LT.0.0: the absolute value of AOPT is a coordinate system ID number (CID on *DEFINE_COORDINATE_NODES, *DEFINE_COORDINATE_SYSTEM or *DEFINE__CO- ORDINATE_VECTOR). XP, YP, ZP Coordinates of point 𝐩 for AOPT = 1. A1, A2, A3 Components of vector 𝐚 for AOPT = 2, for shells and solids. V1, V2, V3 Components of vector 𝐯 for AOPT = 3. D1, D2, D3 Components of vector 𝐝 for AOPT = 2, for solids. The Stoughton non-associated flow rule: In non-associated flow rule, material yield function does not equal to the plastic flow potential. According to Thomas B. Stoughton’s paper titled “A non-associated flow rule for sheet metal forming” in 2002 International Journal of Plasticity 18, 687-714, and “A pressure-sensitive yield criterion under a non-associated flow rule for sheet metal forming” in 2004 International Journal of Plasticity 20, 705-731, plastic potential is defined by: 𝜎̅̅̅̅̅𝑝 = √𝜎11 2 + 𝜆𝑝𝜎22 2 − 2𝜈𝑝𝜎11𝜎22 + 2𝜌𝑝𝜎12 where 𝜎𝑖𝑗 is the stress tensor component; where also, 𝜆𝑝 = 1 + 1 𝑟90 1 + 1 𝑟0 , , 𝜈𝑝 = 𝑟0 1 + 𝑟0 + 1 𝑟0 𝑟90 1 + 1 𝑟0 where 𝑟0, 𝑟45, 𝑟90 are Lankford parameters in the rolling (0°), the diagonal (45°) and the transverse (90°) directions, respectively. + 𝑟45). 𝜌𝑝 = ( Yield function is defined by: 𝜎̅̅̅̅̅𝑦 = √𝜎11 2 + 𝜆𝑦𝜎22 2 − 2𝜈𝑦𝜎11𝜎22 + 2𝜌𝑦𝜎12 where, 𝜆𝑦 = ( 𝜎0 𝜎90 ) , 𝜈𝑦 = 𝜌𝑦 = [1 + 𝜆𝑦 − ( ) 𝜎0 𝜎𝑏 ] , [( ) 2𝜎0 𝜎45 − ( 𝜎0 𝜎𝑏 ) ]. where 𝜎0, 𝜎45, 𝜎90 are the initial yield stresses from uniaxial tension tests in the rolling (0°), the diagonal (45°), and the transverse (90°) directions, respectively. 𝜎𝑏 is the initial yield stress from an equi-biaxial stretching test. The required stress-strain hardening curve must be for uniaxial tension along the rolling direction. Strain rate sensitivity is implemented as an option, by defining a curve (LCIDV) of strain rates vs. stress scale factors, see Figure M260A-2. The variable SCALE is very useful in speeding up the simulation while equalizing the strain rate effect. For example, if the real, physical pulling speed is at 15 mm/s but running at this speed will take a long time, one could increase the pulling speed to 500 mm/s while setting the SCALE to 0.03, resulting in the same results as those from 15 mm/s with the benefit of greatly reduced computational time. See examples in Verification. History variables: 1. Strain rates: history variable #5. 2. Strain rate scale factors: history variable #6. Verification: Uniaxial tension tests were done on a single shell element as shown in Figure M260A-1. Strain rate effect LCIDV is input as shown in Figure M260A-2. In Figure M260A-3, pulling stress vs. strain from various test conditions are compared with input stress- strain curve A. In summary, using the parameter SCALE, the element can be pulled much faster (500 mm/s vs. 15 mm/s) but achieve the same stress vs. strain results, the same strain rates (history variable #5), and the same strain rate scale factor (history variable #6 in Figure M260A-4). Simulation speed can be improved further with increased mass scaling (-1.0*dt2ms) without affecting the results, see Figure M260A-5. A partial keyword input is provided below, for the case with pulling speed of 500 mm/s, strain hardening curve ID of 100, LCIDV curve ID of 105, and strain rate scale factor of 0.03. *KEYWORD *parameter_expression R endtime 0.012 R v 500.0 *CONTROL_TERMINATION $ ENDTIM ENDCYC DTMIN ENDNEG ENDMAS &endtime *MAT_STOUGHTON_NON_ASSOCIATED_FLOW $# mid Ro E PR R00 R45 R90 SIG00 1 7.8000E-9 2.10E05 0.300000 1.1 1.2 1.3 150.4 $ SIG45 SIG90 SIG_B LCIDS LCIDV SCALE 150.1 150.2 150.30 100 105 0.03 $ AOPT 3 $ XP YP ZP A1 A2 A3 $ V1 V2 V3 D1 D2 D3 BETA 1.0 *DEFINE_CURVE 100 0.00000E+00 0.30130E+03 0.10000E-01 0.42295E+03 0.20000E-01 0.47991E+03 0.30000E-01 0.52022E+03 0.40000E-01 0.55126E+03 0.50000E-01 0.57615E+03 ⋮ *DEFINE_CURVE 2-1298 (MAT_248) 105 0.00000E+00 0.10000E+01 0.10000E+00 0.10608E+01 0.50000E+00 0.10828E+01 0.10000E+01 0.10923E+01 *END ⋮ ⋮ Revision information: This material model is available starting in Revision 101821 in explicit, SMP only. The option XUE is available starting on Revision 112711. Fy 0= n i- a x i a l str e s s Fy 0= n str a i n e ll s h Figure M260A-1. Uniaxial tension tests on a single shell element. 1.2 1.15 1.1 1.05 1.0 0.0 LCIDV 1.5 2.0 0.5 1.0 Strain rate (x103) Figure M260A-2. Input LCIDV. 1000 800 600 400 200 ) ( Input Pull speed: 15 mm/s, no LCIDV, SCALE=1.0 Pull speed: 15 mm/s, LCIDV, SCALE=1.0 Pull speed: 500 mm/s, LCIDV, SCALE=1.0 Pull speed: 500 mm/s, LCIDV, SCALE=0.03 0.0 0.2 0.4 0.6 0.8 1.0 Strain ) / ( - # 3.5 3.0 2.5 2.0 1.5 1.0 0.5 0.0 0.03 0.06 0.09 Pull speed: 15 mm/s, LCIDV, SCALE=1.0 Pull speed: 500 mm/s, LCIDV, SCALE=1.0 Pull speed: 500 mm/s, LCIDV, SCALE=0.03 0.1 0.2 Time (sec) 0.3 0.012 100 86 72 58 44 30 15 0.4 Figure M260A-3. Recovered stress-strain curve (top) and strain rates (bottom) under various conditions shown. 1.12 1.1 1.08 1.06 1.04 1.02 - # 1.00 0.0 0.03 0.06 0.09 0.012 1.16 Pull speed: 15 mm/s, LCIDV, SCALE=1.0 Pull speed: 500 mm/s, LCIDV, SCALE=1.0 Pull speed: 500 mm/s, LCIDV, SCALE=0.03 0.1 0.2 Time (sec) 0.3 1.13 1.11 1.08 1.05 1.03 1.00 0.4 Figure M260A-4. Recovered strain rate scale factors under various conditions shown. 1000 800 600 400 200 ) ( Input Pull speed: 500 mm/s, LCIDV, SCALE=0.03, DT2MS=0.0 Pull speed: 500 mm/s, LCIDV, SCALE=0.03, DT2MS=-4E-6 0.0 0.2 0.4 0.6 0.8 1.0 Figure M260A-5. Effect of mass scaling (-1.0*dt2ms). Strain *MAT_MOHR_NON_ASSOCIATED_FLOW_{OPTION} This is Material Type 260B. This material model is implemented based on the papers by Mohr, D., et al.(2010) and Roth, C.C., Mohr, D. (2014). The Johnson-Cook plasticity model of strain hardening, strain rate hardening, and temperature soften effect is modified with a mixed Swift-Voce strain hardening function, coupled with a non- associated flow rule which accounts for the difference between directional dependency of the 𝑟-values (planar anisotropic), and planar isotropic material response of certain Advanced High Strength Steels (AHSS). A ductile fracture model is included based on Hosford-Coulomb fracture initiation model. This model applies to shell elements only. Available options include: <BLANK> XUE Card 1 1 2 Variable MID RO Type A8 F 3 E F 4 5 6 7 8 PR P12 P22 P33 G12 F F F F F Default none none none none none none none none Card 2 1 2 3 4 5 6 7 8 Variable G22 G33 LCIDS LCIDV LCIDT LFLD LFRAC W0 Type F F I I I Default none none none none none I 0 I F none none Card 3 Variable Type 1 A F 2 3 B0 GAMMA F F 4 C F 5 N F 6 7 8 SCALE SIZE0 F F Default none none none none none 1.0 none Card 4 1 2 Variable TREF TMELT Type F F 3 M F 4 5 6 7 8 ETA CP TINI DEPSO DEPSAD F F F F F Default none none none none none none none none Define the following card only for the option XUE: Card 5 1 2 Variable EF0 PLIM Type F F 3 Q F 4 GAMA F 5 M F Default none none none none none 6 7 Card 5 1 2 3 4 5 6 7 8 Variable AOPT Type F Default none Card 6 1 2 3 Variable Type Default Card 7 1 Variable V1 Type F 2 V2 F 3 V3 F Default none none none 7 8 4 A1 F 5 A2 F 6 A3 F none none none 4 5 6 7 8 VARIABLE DESCRIPTION MID RO E PR Material identification. A unique number or label not exceeding 8 characters must be specified. Mass density. Young’s Modulus Poisson’s ratio P12, P22, P33 G12, G22, G33 LCIDS LCIDV LCIDT LFLD LFRAC *MAT_MOHR_NON_ASSOCIATED_FLOW DESCRIPTION Yield function parameters, defined by Lankford parameters in rolling (0°), diagonal (45°) and transverse (90°) directions, respectively; see Non-associated flow rule. Plastic flow potential parameters, defined by Lankford parameters in rolling (0°), diagonal (45°) and transverse (90°) directions, respectively; see Non-associated flow rule. Load curve ID defining stress vs. strain hardening behavior from a uniaxial tension test; must be along the rolling direction. Also see A modified Johnson-Cook. Load curve ID defining stress scale factors vs. strain rates (Figure M260B-1 middle); determined from experiments. Strain rates are stored in history variable #5. Strain rate scale factors are stored in history variable #6. To turn on the variables for viewing in LS- PrePost, set NEIPS to at least “6” in *DATABASE_EXTENT_BI- NARY. It is very useful to know what levels of strain rates, and strain rate scale factors in a particular simulation. Once d3plot files are opened in LS-PrePost, individual element time history can be plotted via menu option Post → History, or a color contour of the entire part can be viewed with the menu option Post → FriComp → Misc. Also see A modified Johnson-Cook. Load curve ID defining stress scale factors vs. temperature in Kelvin (Figure M260B-1 bottom); determined from experiments. Temperatures are stored in history variable #4. Temperature scale factors are stored in history variable #7. To turn on this variable for viewing in LS-PrePost, set NEIPS to at least “7” in *DATABASE_EXTENT_BINARY. It is very useful to know what levels of temperatures and temperature scale factors in a particular simulation. Once d3plot files are opened in LS-PrePost, individual element time history can be plotted via menu option Post → History, or a color contour of the entire part can be viewed with the menu option Post → FriComp → Misc. Also see A modified Johnson-Cook. Load curve ID defining traditional Forming Limit Diagram for linear strain paths. Load curve ID defining a fracture limit curve. Leave this field empty if parameters A, B0, GAMMA, C, N are defined. However, if this field is defined, parameters A, B0, GAMMA, C, N will be ignored even if they are defined. VARIABLE DESCRIPTION W0 Neck (FLD failure) width, typically is the blank thickness. A, B0, GAMMA, C, N SCALE Material parameters for the rate-dependent Hosford-Coulomb fracture initiation model, see Rate-dependent Hosford-Coulomb. This variable can be used to speed up the simulation while equalizing the strain rate effect, useful especially in cases where the pulling speed or punch speed is slow. For example, if the pulling speed is at 15 mm/s but running the simulation at this speed will take a long time, the pulling speed can be increased to 500 mm/s while "SCALE" can be set to 0.03, giving the same results as those from 15 mm/s, but with the benefit of greatly reduced computational time, see examples and Figures in *MAT_260A for details. Furthermore, the increased absolute value (within a reasonable range) of mass scaling -1.0*dt2ms frequently used in forming simulation does not affect the strain rates, as shown in the examples and Figures in *MAT_260A. SIZE0 Fracture gage length used in an experimental measurement, typically between 0.2~0.5mm. TREF, TMELT, M, ETA, CP, TINI, DEPS0, DEPSAD EF0, PLIM, Q, GAMA, M Material parameters to strain temperature. TINI is the initial temperature. See A modified Johnson-Cook for other parameters’ definitions. softening effect due for Material parameters for the option XUE. The parameter k in the original paper is assumed to be 1.0. For details, refer to Xue, L., Wierzbicki, T.’s 2009 paper “Numerical simulation of fracture mode transition in ductile plates” in the International Journal of Solids and Structures. AOPT *MAT_MOHR_NON_ASSOCIATED_FLOW DESCRIPTION Material axes option : EQ.0.0: EQ.2.0: EQ.3.0: LT.0.0: locally orthotropic with material axes determined by element nodes 1, 2, and 4, as with *DEFINE_- COORDINATE_NODES, and then rotated about the shell element normal by the angle BETA. globally orthotropic with material axes determined by the vector 𝐚 for shells, as with *DEFINE_COOR- DINATE_VECTOR. locally orthotropic material axes determined by rotating the material axes about the element nor- mal by an angle, BETA, from a line in the plane of the element defined by the cross product of the vector 𝐯 with the element normal. the absolute value of AOPT is a coordinate system ID number (CID on *DEFINE_COORDINATE_- NODES, *DEFINE_COORDINATE_SYSTEM or *DEFINE__COORDINATE_VECTOR). A1, A2, A3 Components of vector 𝐚 for AOPT = 2. V1, V2, V3 Components of vector 𝐯 for AOPT = 3. Non-associated flow rule: Referring to Mohr, D., Dunand, M., and Kim, K-H.’s 2010 and 2014 papers in the International Journal of Plasticity, Hill’s 1948 quadratic yield function is written as: where 𝝈 is the Cauchy stress tensor and 𝝈 the equivalent stress is defined by: 𝑓 (𝝈, 𝑘) = 𝜎̅̅̅̅̅ − 𝑘 = 0 𝜎̅̅̅̅̅ = √(𝐏𝝈) ∙ 𝝈 Where 𝐏 is a symmetric positive-definite matrix defined through three independent parameters P12, P22, P33: 𝐏 = P12 ⎡ P12 P22 ⎢ ⎣ ⎤ ⎥ P33⎦ Flow rule, which defines the incremental plastic strain tensor, is written as follows: 𝑑𝛆𝑝 = 𝑑𝛿 𝜕𝑔(𝝈) 𝜕𝝈 where 𝑑𝛿 is a scalar plastic multiplier. The plastic potential function 𝑔(𝝈) can be defined as a quadratic function in stress space: with, 𝑔(𝝈) = √(𝐆𝝈) ∙ 𝝈 𝐆 = G12 G12 G22 ⎡ ⎢ ⎣ ⎤ ⎥ G33⎦ When 𝐏𝐆, it leads to non-associated flow rule. For example, 𝐏 can represent isotropic von-Mises yield surface by setting P11 = P22 = 1.0, P12 = −0.5, P33 = 3.0. 𝐆 can represent an orthotropic plastic flow potential by setting: 𝐺12 = 𝐺22 = 𝐺33 = , 𝑟0 1 + 𝑟0 𝑟0(1 + 𝑟90) 𝑟90(1 + 𝑟0) (1 + 2𝑟45)(𝑟0 + 𝑟90) 𝑟90(1 + 𝑟0) , . where 𝑟0, 𝑟45, 𝑟90 are Lankford coefficients in the rolling, diagonal and transverse direction. Experiments have shown on the stress level, some AHSS, e.g., DP590, and TRIP780 show strong directional dependency of 𝑟-values, while nearly the same stress- strain curves have been measured in all directions. The directional dependency of 𝑟- values suggests planar anisotropy while the material response on the stress level is planar isotropic, which is the main reason to employ the non-associated flow rule. On the other hand, if 𝐏 = 𝐆, the associated flow rule is recovered. A modified Johnson-Cook plasticity model with mixed Swift-Voce hardening: The Johnson-Cook plasticity model (1983) multiplicatively decomposes the deformation resistance into three functions representing the effect of strain hardening, strain rate and temperature. The Johnson-Cook model is modified to include hardening saturation with a mixed Swift-Voce hardening law (Sung et al, A plastic constitutive equation incorporating strain, strain-rate, and temperature, International Journal of Plasticity, 2010), which gives a better description of the hardening at large strain levels, thus improving the prediction of the necking and post-necking response of metal sheet: 𝜎𝑦 = (𝛼(𝐴(𝜀̅𝑝𝑙 + 𝜀0) ) + (1 − 𝛼) (𝑘0 + 𝑄(1 − 𝑒−𝛽𝜀̅𝑝𝑙))) 1 + 𝐶𝑙𝑛 ⎜⎜⎜⎛ ⎝ 𝜀̇𝑝𝑙 ⎟⎞ 𝜀0̇ ⎠ ⎜⎛ ⎝ ⎟⎟⎟⎞ ⎠ (1 − ( 𝑇 − 𝑇𝑟 𝑇𝑚 − 𝑇𝑟 ) ) where 𝜀̅𝑝𝑙 and 𝜀̇𝑝𝑙 are effective plastic strain and strain rate, respectively; 𝑇𝑚 (TMELT), 𝑇𝑟 (TREF) and 𝑇 are the melting temperature, reference temperature (ambient temperature 293 kelvin) and current temperature, respectively; 𝑚 (M) is an exponent coefficient. For other symbols’ definitions refer to the aforementioned paper. To make this material model more general and flexible, three load curves are used to define the three components of the deformation resistance. A load curve (LCIDS) is used to describe the strain hardening: LCIDS: (𝛼(𝐴(𝜀̅𝑝𝑙 + 𝜀0) ) + (1 − 𝛼) (𝑘0 + 𝑄(1 − 𝑒−𝛽𝜀̅𝑝𝑙))) Strain rate is described by a load curve LCIDV (stress scale factor vs. strain rates, Figure M260B-1 middle), which scales the stresses based on the strain rates during a simulation: LCIDV: (1 + 𝐶𝑙𝑛 ( 𝑝𝑙 𝜀̇ 𝜀0̇ )) The temperature softening effect is defined by another load curve LCIDT (stress scale factor vs. temperature, Figure M260B-1 bottom), which scales the stresses based on the temperatures during the simulation: LCIDT: (1 − ( 𝑇−𝑇𝑟 𝑇𝑚−𝑇𝑟 ) ) The temperature effect is a self-contained model, in other words, it does not require thermal exchange with the environment, and it calculates temperatures based on plastic strain and strain rate. The temperature evolution is determined with: 𝜂𝑘 𝜌𝐶𝑝 𝑑𝑇 = 𝜔[𝜀̇𝑝𝑙] 𝜎̅̅̅̅̅𝑑𝜀̅𝑝𝑙 Where 𝜂𝑘 (ETA) is Taylor-Quinney coefficient, 𝜌 (R0) is the mass density and 𝐶𝑝 (CP) is the heat capacity; also where, 𝜔[𝜀̇𝑝𝑙] = (𝜀̇ ⎧ {{{{ {{{{ ⎨ ⎩ 𝑓𝑜𝑟 𝜀̇𝑝𝑙 < 𝜀̇𝑖𝑡 𝑝𝑙−𝜀̇𝑖𝑡) (3𝜀̇𝑎−2𝜀̇ (𝜀̇𝑎−𝜀̇𝑖𝑡)3 𝑝𝑙−𝜀̇𝑖𝑡) 𝑓𝑜𝑟 𝜀̇𝑖𝑡 ≤ 𝜀̇𝑝𝑙 ≤ 𝜀̇𝑎 𝑓𝑜𝑟 𝜀̇𝑎 < 𝜀̇𝑝𝑙 where 𝜀̇𝑖𝑡 > 0 and 𝜀̇𝑎 > 𝜀̇𝑖𝑡 define the limits of the respective domains of isothermal and adiabatic conditions (𝜀̇𝑎 = DEPSAD). For simplification, 𝜀̇𝑖𝑡 = 𝜀̇0(DEPS0). As shown in a single shell element uniaxial stretching (Figure M260B-1), the general effect of the LCIDV is to elevate the strain hardening behavior as the strain rate increases (curve “D” in Figure M260B-2 top), while the effect of the LCIDT is strain softening as temperature rises (curve “C” in Figure M260B-2 top). A combined effect of both LCIDV and LCIDT may result in strain hardening initially before temperature rise enough to cause the strain softening in the model (curve “E” in Figure M260B-2 top). The temperature and strain rates calculated for each element can be viewed with history variables #4 and #5 (curves “C” and “D” in Figure M260B-2 bottom), respectively, while the strain rate scale factors and temperature scale factors can be viewed with history variable #6 and #7, respectively. Rate-dependent Hosford-Coulomb fracture initiation model: An extension of the Hosford-Coulomb fracture initiation model is used to account for the effect of strain rate on ductile fracture. The damage accumulation is calculated through history variable #3, and fracture occurs at an equivalent plastic strain 𝜀̅𝑓 when the variable reaches 1.0: 𝜀𝑓 ∫ 𝑑𝜀̅𝑝𝑙 𝑝𝑟[𝜂, 𝜃̅] 𝜀̅𝑓 = 1 𝑝𝑟, 𝜂, 𝜃̅ are strain to fracture, stress triaxiality and the Lode parameter, Where 𝜀̅𝑓 respectively. The fracture parameters A, B0, GAMMA, C, N (𝑎, 𝑏0, 𝛾, 𝑐, 𝑛) are indicated in the following equations. Strain to fracture for proportional load: 𝑝𝑟[𝜂, 𝜃̅] = 𝑏(1 + 𝑐) 𝜀̅𝑓 { ⎜⎜⎜⎜⎜⎛ ⎝ ((𝑓1 − 𝑓2)𝑎 + (𝑓2 − 𝑓3)𝑎 + (𝑓1 − 𝑓3)𝑎)} + 𝑐(2𝜂 + 𝑓1 + 𝑓3) −1 ⎟⎟⎟⎟⎟⎞ ⎠ where 𝑎 is the Hosford exponent, 𝑐 is the friction coefficient controlling the effect of triaxiality, 𝑛 is the stress state sensitivity. The Lode angle parameter dependent trigonometric functions: 𝑓1[𝜃̅] = 2 3 cos[𝜋 and coefficient 𝑏 (strain to fracture for uniaxial or equi-biaxial stretching): 6 (3 + 𝜃̅)], 𝑓3[𝜃̅] = − 2 6 (1 − 𝜃̅)], 𝑓2[𝜃̅] = 2 3 cos[𝜋 3 cos[𝜋 6 (1 + 𝜃̅)] 𝑏 = {⎧ ⎩{⎨ 𝑏0 𝑏0 (1 + 𝛾𝑙𝑛 [ 𝜀̇𝑝 𝜀̇0 ]) 𝑓𝑜𝑟 𝜀̇𝑝 < 𝜀̇0 𝑓𝑜𝑟 𝜀̇𝑝 > 𝜀̇0 where 𝛾 is the strain rate sensitivity. Corresponding parameters summary: The following table lists variable names used in this material model and corresponding symbols employed in the papers: P12 P22 P33 G12 G22 G33 A B0 GAMMA C N P12 P22 P33 𝐺12 𝐺22 𝐺33 𝑎 𝑏0 𝛾 𝑐 𝑛 TREF TMELT M ETA CP DEPSO DEPSAD R0 𝑇𝑟 𝑇𝑚 𝑚 𝜂𝑘 𝐶𝑝 𝜀̇𝑖𝑡/𝜀̇0 𝜀̇𝑎 𝜌 History variables summary: 1. Damage accumulation: history variable #3. Elements will be deleted if this variable reaches 1.0 for more than half of the through-thickness integration points (Revision 109792). 2. Temperatures: history variable #4. 3. Strain rates: history variable #5. 4. Strain rate scale factors: history variable #6. 5. Temperature scale factor: history variable #7. Keyword example input: A sample material input card can be found below, with parameters from Mohr, D., et al.(2010) and Roth, C.C., Mohr, D. (2014). *MAT_MOHR_NON_ASSOCIATED_FLOW $# mid R0 E PR P12 P22 P33 G12 1 7.8000E-9 2.10E05 0.300000 -0.5 1.0 3.0 -0.4946 $ G22 G33 LCIDS LCIDV LCIDT LFLD LFRAC W0 0.9318 2.4653 100 105 102 $ A B0 GAMMA C N SCALE 1.97 0.82 0.025 0.00 0.199 3.132E-3 $ TREF TMELT M ETA CP TINI DEPSO DEPSAD 293.0 1673.70 0.921 0.9 420.0 293.0 0.001164 1.379 $ AOPT 3 $ XP YP ZP A1 A2 A3 $ V1 V2 V3 D1 D2 D3 BETA 1.0 *DEFINE_CURVE 100 0.00000E+00 0.30130E+03 0.10000E-01 0.42295E+03 0.20000E-01 0.47991E+03 0.30000E-01 0.52022E+03 0.40000E-01 0.55126E+03 ⋮ ⋮ *DEFINE_CURVE 105 0.00000E+00 0.10000E+01 0.10000E+00 0.10608E+01 0.50000E+00 0.10828E+01 0.10000E+01 0.10923E+01 ⋮ ⋮ *DEFINE_CURVE 102 0.29300E+03 0.10000E+01 0.33300E+03 0.96168E+00 0.37300E+03 0.92744E+00 0.41300E+03 0.89459E+00 0.45300E+03 0.86261E+00 ⋮ ⋮ Revision information: This material model is available in SMP starting in Revision 102375. Revision history is listed below: 1) Element deletion feature based on damage accumulation: Revision 109792. 2) The option XUE is available starting on Revision 111531. U n s i n e d s h e Fy 0= a x i a l - U n i Fy 0= 1.2 1.15 1.1 1.05 1.0 0.0 1.0 0.8 0.6 0.4 0.2 LCIDV 0.5 1.0 Strain rate (x103) 1.5 2.0 LCIDT 0.0 0.4 0.6 0.8 1.0 1.2 1.4 Temperature (x103 kelvin) Figure M260B-1. Uniaxial stretching on a single shell element; Input curves LCIDV and LCIDT. Pull speed: 15 mm/s, SCALE=1.0 1000 800 600 400 200 ) ( Input no LCIDV, no LCIDT no LCIDV, with LCIDT with LCIDV, no LCIDT with LCIDV, with LCIDT 0.0 0.2 0.4 0.6 0.8 1.0 Strain 3.0 2.5 2.0 1.5 1.0 0.5 0.0 ) / ( - # Pull speed: 15 mm/s, SCALE=1.0 0.1 0.2 Time (sec) 0.3 500 450 400 350 300 ) ( - # 250 0.4 Figure M260B-2. Results of a single element uniaxial stretching - stress-strain curves (top), strain rates and temperature history under various conditions. *MAT_LAMINATED_FRACTURE_DAIMLER_PINHO This is Material Type 261 which is an orthotropic continuum damage model for laminated fiber-reinforced composites. See Pinho, Iannucci and Robinson [2006]. It is based on a physical model for each failure mode and considers non-linear in-plane shear behavior. This model is implemented for shell, thick shell and solid elements. Remark: Laminated shell theory can be applied by setting LAMSHT ≥ 3 in *CON- TROL_SHELL. Card 1 1 Variable MID Type A8 Card 2 1 2 RO F 2 3 EA F 3 4 EB F 4 5 EC F 5 6 7 8 PRBA PRCA PRCB F 6 F 7 F 8 Variable GAB GBC GCA AOPT DAF DKF DMF EFS Type F F F F F F Card 3 Variable 1 XP Type F Card 4 Variable 1 V1 Type F 2 YP F 2 V2 F 3 ZP F 3 V3 F 4 A1 F 4 D1 F 5 A2 F 5 D2 F F 7 F 8 7 8 6 A3 F 6 D3 MANGLE F Card 5 1 2 3 4 5 6 7 8 Variable ENKINK ENA ENB ENT ENL Type F F F F F Card 6 Variable 1 XC Type F Card 7 1 2 XT F 2 3 YC F 3 4 YT F 4 5 SL F 5 6 7 8 Variable FIO SIGY LCSS BETA PFL PUCK SOFT Type F F F F F F F VARIABLE DESCRIPTION 6 7 8 DT F MID RO EA EB EC PRBA PRCA PRCB GAB GBC Material identification. A unique number or label not exceeding 8 characters must be specified. Mass density 𝐸𝑎, Young’s modulus in 𝑎-direction (longitudinal) 𝐸𝑏, Young’s modulus in 𝑏-direction (transverse) 𝐸𝑐, Young’s modulus in 𝑐-direction 𝜈𝑏𝑎, Poisson’s ratio 𝑏𝑎 𝜈𝑐𝑎, Poisson’s ratio 𝑐𝑎 𝜈𝑐𝑏, Poisson’s ratio 𝑐𝑏 𝐺𝑎𝑏, shear modulus 𝑎𝑏 𝐺𝑏𝑐, shear modulus 𝑏𝑐 GCA AOPT *MAT_LAMINATED_FRACTURE_DAIMLER_PINHO DESCRIPTION 𝐺𝑐𝑎, shear modulus 𝑐𝑎 Material axes option : EQ.0.0: locally orthotropic with material axes determined by element nodes 1, 2, and 4, as with *DEFINE_COORDI- NATE_NODES, and then, for shells only, rotated about the shell element normal by an angle MANGLE. EQ.1.0: locally orthotropic with material axes determined by a point in space and the global location of the element center; this is the 𝑎-direction. This option is for solid elements only. EQ.2.0: globally orthotropic with material axes determined by vectors defined below, as with *DEFINE_COORDI- NATE_VECTOR. EQ.3.0: locally orthotropic material axes determined by rotating the material axes about the element normal by an angle (MANGLE) from a line in the plane of the el- ement defined by the cross product of the vector v with the element normal. EQ.4.0: locally orthotropic in cylindrical coordinate system with the material axes determined by a vector 𝐯, and an originating point, 𝐩, which define the centerline ax- is. This option is for solid elements only. LT.0.0: the absolute value of AOPT is a coordinate system ID number (CID on *DEFINE_COORDINATE_NODES, *DEFINE_COORDINATE_SYSTEM or *DEFINE_CO- ORDINATE_VECTOR). Available in R3 version of 971 and later. DAF Flag to control failure of an longitudinal (fiber) tensile failure: integration point based on EQ.0.0: IP fails if any damage variable reaches 1.0. EQ.1.0: no failure of IP due to fiber tensile failure. This condition corresponds to history variable “da(i)” reaching 1.0 VARIABLE DKF DESCRIPTION Flag to control failure of an longitudinal (fiber) compressive failure: integration point based on EQ.0.0: IP fails if any damage variable reaches 1.0. EQ.1.0: no failure of IP due to fiber compressive failure. This condition corresponds to history variable “dkink(i)” reaching 1.0. DMF Flag to control failure of an integration point based on transverse (matrix) failure: EQ.0.0: IP fails if any damage variable reaches 1.0. EQ.1.0: no failure of IP due to matrix failure. This condition corresponds to history variable “dmat(i)” reaching 1.0. EFS Maximum effective strain for element layer failure. A value of unity would equal 100% strain. GT.0.0: fails when effective strain calculated assuming material is vol-ume preserving exceeds EFS. LT.0.0: fails when effective strain calculated from the full strain tensor exceeds |EFS|. XP, YP, ZP Coordinates of point p for AOPT = 1 and 4. A1, A2, A3 Define components of vector 𝐚 for AOPT = 2. V1, V2, V3 Define components of vector 𝐯 for AOPT = 3. D1, D2, D3 Define components of vector 𝐝 for AOPT = 2. MANGLE Material angle in degrees for AOPT = 0 (shells only) and AOPT = 3. MANGLE may be overridden on the element card, see *ELEMENT_SHELL_BETA and *ELEMENT_SOLID_ORTHO. ENKINK Fracture toughness for longitudinal (fiber) compressive failure mode. GT.0.0: The given value will be regularized with the characteristic element length. LT.0.0: Load curve ID = (-ENKINK) which defines the fracture toughness for fiber compressive failure mode as a func- tion of characteristic element length. No further regu- larization. *MAT_LAMINATED_FRACTURE_DAIMLER_PINHO DESCRIPTION ENA Fracture toughness for longitudinal (fiber) tensile failure mode. GT.0.0: The given value will be regularized with the characteristic element length. LT.0.0: Load curve ID = (-ENA) which defines the fracture toughness for fiber tensile failure mode as a function of characteristic element length. No further regulariza- tion. ENB Fracture toughness for intralaminar matrix tensile failure. GT.0.0: The given value will be regularized with the characteristic element length. LT.0.0: Load curve ID = (-ENB) which defines the fracture toughness for intralaminar matrix tensile failure as a function of characteristic element length. No further regularization. ENT Fracture toughness for intralaminar matrix transverse shear failure. GT.0.0: The given value will be regularized with the characteristic element length. LT.0.0: Load curve ID = (-ENT) which defines the fracture toughness for intralaminar matrix transverse shear failure as a function of characteristic element length. No further regularization. ENL Fracture toughness for intralaminar matrix longitudinal shear failure. GT.0.0: The given value will be regularized with the characteristic element length. LT.0.0: Load curve ID = (-ENL) which defines the fracture toughness for intralaminar matrix longitudinal shear failure as a function of characteristic element length. No further regularization. XC Longitudinal compressive strength, 𝑎-axis (positive value). GT.0.0: constant value LT.0.0: Load curve ID = (-XC) which defines the longitudinal compressive strength vs. longitudinal strain rate (𝜖 ̇𝑎𝑎). VARIABLE DESCRIPTION XT Longitudinal tensile strength, 𝑎-axis. GT.0.0: constant value LT.0.0: Load curve ID = (-XT) which defines the longitudinal tensile strength vs. longitudinal strain rate (𝜖 ̇𝑎𝑎). YC Transverse compressive strength, 𝑏-axis (positive value). GT.0.0: constant value LT.0.0: Load curve ID = (-YC) which defines the transverse compressive strength vs. transverse strain rate (𝜖 ̇𝑏𝑏). YT Transverse tensile strength, 𝑏-axis. GT.0.0: constant value LT.0.0: Load curve ID = (-YT) which defines the transverse tensile strength vs. tansverse strain rate (𝜖 ̇𝑏𝑏). SL Longitudinal shear strength. GT.0.0: constant value LT.0.0: Load curve ID = (-SL) which defines the longitudinal shear strength vs. in-plane shear strain rate (𝜖 ̇𝑎𝑏). FIO Fracture angle in pure transverse compression (in degrees, default = 53.0). SIGY In-plane shear yield stress. *MAT_LAMINATED_FRACTURE_DAIMLER_PINHO DESCRIPTION LCSS Load curve ID or Table ID. Load Curve. When LCSS is a Load curve ID, it defines the non- linear in-plane shear-stress as a function of in-plane shear-strain. Tabular Data. The table maps in-plane strain rate values (𝜖 ̇𝑎𝑏) to a load curve giving the in-plane shear-stress as a function of in- plane shear-strain. For strain rates below the minimum value, the curve for the lowest defined value of strain rate is used. Likewise, when the strain rate exceeds the maximum value, the curve for the highest defined value of strain rate is used. Logarithmically Defined Table. If the first curve in the table corresponds to a negative strain rate, LS-DYNA assumes that the natural logarithm of the strain rate value is used for all stress- strain curves. Since the tables are internally discretized to equally spaced points, natural logarithms are necessary, for example, if the curves correspond to rates from 10−4 to 104. Computing natural logarithms can substantially increase the computational time on certain computer architectures BETA Hardening parameter for in-plane shear plasticity (0.0 ≤ BETA ≤ 1.0). EQ.0.0: EQ.1.0: Pure kinematic hardening Pure isotropic hardening 0.0 < BETA < 1.0: mixed hardening. PFL Percentage of layers which must fail until crashfront is initiated. E.g. |PFL| = 80.0, then 80% of layers must fail until strengths are reduced in neighboring elements. Default: all layers must fail. A single layer fails if 1 in-plane IP fails (PFL > 0) or if 4 in-plane IPs fail (PFL < 0). PUCK Flag for evaluation and post-processing of Puck’s inter-fiber- failure criterion (IFF, see Puck, Kopp and Knops [2002]). EQ.0.0: no evaluation of Puck’s IFF-criterion. EQ.1.0: Puck’s IFF-criterion will be evaluated. SOFT Softening reduction factor for material strength in crashfront elements (default = 1.0). am −σ cψ c ψ −σ bψ −σ bc bc −σ −σ cb cb −σ bm bψ cψ −σ bψ bψ ma c ψ Matrix fracture plane −σ cψ bψ mb mb Figure M261-1. Definition of angles and stresses in fracture plane VARIABLE DESCRIPTION DT Strain rate averaging option. EQ.0.0: Strain rate is evaluated using a running average. LT.0.0: Strain rate is evaluated using average of last 11 time steps. GT.0.0: Strain rate is averaged over the last DT time units. Remarks: Failure Surfaces The failure surface to limit the elastic domain is assembled by four sub-surfaces, representing different failure mechanisms. See Figure M261-1 for definition of angles. They are defined as follows: 1. longitudinal (fiber) tension, 𝑓𝑎 = 𝜎𝑎 𝑋𝑇 = 1 2. longitudinal (fiber) compression (3D-kinking model) – (transformation to fracture plane), ) + ( 𝑓𝑘𝑖𝑛𝑘 = ⎧ {{{ ⎨ {{{ ⎩ ( 𝜏𝑇 𝑆𝑇 − 𝜇𝑇𝜎𝑛 𝜎𝑛 𝑌𝑇 ) ( + ( 𝜏𝑇 𝑆𝑇 𝜏𝐿 𝑆𝐿 − 𝜇𝐿𝜎𝑛 ) + ( ) ) = 1 𝑖𝑓 𝜎𝑏𝑚 ≤ 0 = 1 𝑖𝑓 𝜎𝑏𝑚 > 0 𝜏𝐿 𝑆𝐿 LS-DYNA R10.0 Figure M261-2. Damage evolution law 𝑆𝑇 = 𝜎𝑛 = 𝑌𝐶 2 tan(𝜙0) 𝜎𝑏𝑚 + 𝜎𝑐𝜓 ; 𝜇𝑇 = − tan(2𝜙0) ; 𝜇𝐿 = 𝑆𝐿 𝜇𝑇 𝑆𝑇 + 𝜎𝑏𝑚 − 𝜎𝑐𝜓 cos(2𝜙) + 𝜏𝑏𝑚𝑐𝜓 sin(2𝜙) 𝜏𝑇 = − 𝜎𝑏𝑚 − 𝜎𝑐𝜓 sin(2𝜙) + 𝜏𝑏𝑚𝑐𝜓 cos(2𝜙) 𝜏𝐿 = 𝜏𝑎𝑚𝑏𝑚 cos(𝜙) + 𝜏𝑐𝜓𝑎𝑚 sin(𝜙) 3. transverse (matrix) failure: transverse tension, 𝑓𝑚𝑎𝑡 = ( 𝜎𝑛 𝑌𝑇 ) + ( 𝜏𝑇 𝑆𝑇 ) + ( ) 𝜏𝐿 𝑆𝐿 = 1 𝑖𝑓 𝜎𝑛 ≥ 0 with 𝜎𝑛 = + 𝜎𝑏 + 𝜎𝑐 𝜎𝑏 − 𝜎𝑐 𝜎𝑏 − 𝜎𝑐 cos(2𝜙) + 𝜏𝑏𝑐 sin(2𝜙) sin(2𝜙) + 𝜏𝑏𝑐 cos(2𝜙) 𝜏𝑇 = − 𝜏𝐿 = 𝜏𝑎𝑏 cos(𝜙) + 𝜏𝑐𝑎 sin(𝜙) 4. transverse (matrix) failure: transverse compression/shear, 𝑓𝑚𝑎𝑡 = ( 𝜏𝑇 𝑆𝑇 − 𝜇𝑇𝜎𝑛 ) + ( 𝜏𝐿 𝑆𝐿 − 𝜇𝐿𝜎𝑛 ) = 1 𝑖𝑓 𝜎𝑛 < 0 Remarks: Damange Evolution: As long as the stress state is located within the failure surface the model behaves orthotropic elastic. When reaching the failure criteria the effective (undamaged) stresses will be reduced by a factor of (1 − 𝑑), where the damage variable d represents failure mechanisms one of the damage variables defined the different for non-linearity defined via *DEFINE_CURVE Figure M261-3. Definition of non-linear in-plane shear behavior (𝑑da, 𝑑kink, 𝑑mat). The growth of these damage variables is driven by a linear damage evolution law based on fracture toughnesses (𝛤 → ENKINK, ENA, ENB, ENT, ENL) and a characteristic internal element length, 𝐿, to account for objectivity. See Figure M261-2. Remarks: Nonlinear In-Plane Shear: To account for the characteristic non-linear in-plane shear behavior of laminated fiber- reinforced composites a 1D elasto-plastic formulation is coupled to a linear damage behavior once the maximum allowable stress state for shear failure is reached. The non- linearity of the shear behavior can be introduced via the definition of an explicit shear stress vs. engineering shear strain curve (LCSS) with *DEFINE_CURVE. See Figure M261-3 (in which epsilon designates engineering shear strain rather than tensorial shear strain). Remarks: References: More detailed information about this material model can be found in Pinho, Iannucci and Robinson [2006]. Remarks: Element Deletion: When failure has occurred in all the composite layers (through-thickness integration points), the element is deleted. Elements which share nodes with the deleted element become “crashfront” elements and can have their strengths reduced by using the SOFT parameter. An earlier initiation of crashfront elements is possible by using the parameter PFL. Remarks: History Variables: The number of additional integration point variables written to the LS-DYNA database is input by the *DATABASE_EXTENT_BINARY definition with the variable NEIPS (shells) and NEIPH (solids). These additional variables are tabulated below (i = integration point): History Variable Description Value LS-PrePost history variable fa(i) fkink(i) fmat(i) matrix mode fiber tensile mode fiber compressive mode 0 → 1: elastic 1: failure criterion rea- ched da(i) dkink(i) damage fiber tension damage compression fiber dmat(i) damage transverse dam(i) crashfront fmt_p(i) fmc_p(i) theta_p(i) tensile matrix mod (Puck criteria) compressive mode (Puck criteria) angle of fracture plane (radians, Puck criteria) matrix 0: elastic 1: fully damaged -1: element intact 10 - 8: element in crashfront +1: element failed 0 → 1: elastic 1: failure criterion rea- ched 1 2 3 4 5 6 7 8 9 10 11 12 *MAT_LAMINATED_FRACTURE_DAIMLER_CAMANHO This is Material Type 262 which is an orthotropic continuum damage model for laminated fiber-reinforced composites. See Maimí, Camanho, Mayugo and Dávila [2007]. It is based on a physical model for each failure mode and considers a simplified non-linear in-plane shear behavior. This model is implemented for shell, thick shell and solid elements. NOTE: Laminated shell theory can be applied by setting LAMSHT ≥ 3 in *CONTROL_SHELL. Card 1 1 Variable MID Type A8 Card 2 1 2 RO F 2 3 EA F 3 4 EB F 4 5 EC F 5 6 7 8 PRBA PRCA PRCB F 6 F 7 F 8 Variable GAB GBC GCA AOPT DAF DKF DMF EFS Type F F F F F F Card 3 Variable 1 XP Type F Card 4 Variable 1 V1 Type F 2 YP F 2 V2 F 3 ZP F 3 V3 F 4 A1 F 4 D1 F 5 A2 F 5 D2 F F 7 F 8 7 8 6 A3 F 6 D3 MANGLE F Card 5 1 2 3 4 5 6 7 8 Variable GXC GXT GYC GYT GSL GXCO GXTO Type F F F F F Card 6 Variable 1 XC Type F Card 7 1 2 XT F 2 3 YC F 3 4 YT F 4 5 SL F 5 F 6 F 7 XCO XTO F 6 F 7 Variable FIO SIGY ETAN BETA PFL PUCK SOFT Type F F F F F F F 8 8 DT F VARIABLE DESCRIPTION MID RO EA EB EC PRBA PRCA PRCB GAB GBC Material identification. A unique number or label not exceeding 8 characters must be specified. Mass density 𝐸𝑎, Young’s modulus in 𝑎-direction (longitudinal) 𝐸𝑏, Young’s modulus in 𝑏-direction (transverse) 𝐸𝑐, Young’s modulus in 𝑐-direction 𝜈𝑏𝑎, Poisson’s ratio 𝑏𝑎 𝜈𝑐𝑎, Poisson’s ratio 𝑐𝑎 𝜈𝑐𝑏, Poisson’s ratio 𝑐𝑏 𝐺𝑎𝑏, shear modulus 𝑎𝑏 𝐺𝑏𝑐, shear modulus 𝑏𝑐 VARIABLE DESCRIPTION GCA AOPT 𝐺𝑐𝑎, shear modulus 𝑐𝑎 Material axes option : EQ.0.0: locally orthotropic with material axes determined by element nodes 1, 2, and 4, as with *DEFINE_COORDI- NATE_NODES, and then, for shells only, rotated about the shell element normal by an angle MANGLE. EQ.1.0: locally orthotropic with material axes determined by a point in space and the global location of the element center; this is the 𝑎-direction. This option is for solid elements only. EQ.2.0: globally orthotropic with material axes determined by vectors defined below, as with *DEFINE_COORDI- NATE_VECTOR. EQ.3.0: locally orthotropic material axes determined by rotating the material axes about the element normal by an angle (MANGLE) from a line in the plane of the el- ement defined by the cross product of the vector v with the element normal. EQ.4.0: locally orthotropic in cylindrical coordinate system with the material axes determined by a vector 𝐯, and an originating point, 𝐩, which define the centerline ax- is. This option is for solid elements only. LT.0.0: the absolute value of AOPT is a coordinate system ID number (CID on *DEFINE_COORDINATE_NODES, *DEFINE_COORDINATE_SYSTEM or *DEFINE_CO- ORDINATE_VECTOR). Available in R3 version of 971 and later. DAF Flag to control failure of an longitudinal (fiber) tensile failure: integration point based on EQ.0.0: IP fails if any damage variable reaches 1.0. EQ.1.0: no failure of IP due to fiber tensile failure, da(i)=1.0 DKF *MAT_LAMINATED_FRACTRURE_DAIMLER_CAMANHO DESCRIPTION Flag to control failure of an longitudinal (fiber) compressive failure: integration point based on EQ.0.0: IP fails if any damage variable reaches 1.0. EQ.1.0: no failure of IP due to fiber compressive failure, dkink(i) = 1.0. DMF Flag to control failure of an integration point based on transverse (matrix) failure: EQ.0.0: IP fails if any damage variable reaches 1.0. EQ.1.0: no failure of IP due to matrix failure, dmat(i)=1.0 EFS Maximum effective strain for element layer failure. A value of unity would equal 100% strain. GT.0.0: fails when effective strain calculated assuming material is vol-ume preserving exceeds EFS. LT.0.0: fails when effective strain calculated from the full strain tensor exceeds |EFS|. XP YP ZP Coordinates of point 𝐩 for AOPT = 1 and 4. A1 A2 A3 Define components of vector 𝐚 for AOPT = 2. V1 V2 V3 Define components of vector 𝐯 for AOPT = 3. D1 D2 D3 Define components of vector 𝐝 for AOPT = 2. MANGLE Material angle in degrees for AOPT = 0 (shells only) and AOPT = 3. MANGLE may be overridden on the element card, see *ELEMENT_SHELL_BETA and *ELEMENT_SOLID_ORTHO. GXC Fracture toughness for longitudinal (fiber) compressive failure mode. GT.0.0: The given value will be regularized with the characteristic element length. LT.0.0: Load curve ID = (-GXC) which defines the fracture toughness for fiber compressive failure mode as a func- tion of characteristic element length. No further regu- larization. VARIABLE DESCRIPTION GXT Fracture toughness for longitudinal (fiber) tensile failure mode. GT.0.0: The given value will be regularized with the characteristic element length. LT.0.0: Load curve ID = (-GXT) which defines the fracture toughness for fiber tensile failure mode as a function of characteristic element length. No further regulariza- tion. GYC Fracture toughness for transverse compressive failure mode. GT.0.0: The given value will be regularized with the characteristic element length. LT.0.0: Load curve ID = (-GYC) which defines the fracture toughness for transverse compressive failure mode as a function of characteristic element length. No further regularization. GYT Fracture toughness for transverse tensile failure mode. GT.0.0: The given value will be regularized with the characteristic element length. LT.0.0: Load curve ID = (-GYT) which defines the fracture toughness for transverse tensile failure mode as a func- tion of characteristic element length. No further regu- larization. GSL Fracture toughness for in-plane shear failure mode. GT.0.0: The given value will be regularized with the characteristic element length. LT.0.0: Load curve ID = (-GSL) which defines the fracture toughness for in-plane shear failure mode as a function of characteristic element length. No further regulariza- tion. GXCO *MAT_LAMINATED_FRACTRURE_DAIMLER_CAMANHO DESCRIPTION Fracture toughness for longitudinal (fiber) compressive failure mode to define bi-linear damage evolution. GT.0.0: The given value will be regularized with the characteristic element length. LT.0.0: Load curve ID = (-GXCO) which defines the fracture toughness for fiber compressive failure mode to define bi-linear damage evolution as a function of characteris- tic element length. No further regularization. GXTO Fracture toughness for longitudinal (fiber) tensile failure mode to define bi-linear damage evolution. GT.0.0: The given value will be regularized with the characteristic element length. LT.0.0: Load curve ID = (-GXTO) which defines the fracture toughness for fiber tensile failure mode to define bi- linear damage evolution as a function of characteristic element length. No further regularization. XC Longitudinal compressive strength, 𝑎-axis (positive value). GT.0.0: constant value LT.0.0: Load curve ID = (-XC) which defines the longitudinal compressive strength vs. longitudinal strain rate (𝜖 ̇𝑎𝑎). XT Longitudinal tensile strength, 𝑎-axis. GT.0.0: constant value LT.0.0: Load curve ID = (-XT) which defines the longitudinal tensile strength vs. longitudinal strain rate (𝜖 ̇𝑎𝑎). YC Transverse compressive strength, 𝑏-axis (positive value). GT.0.0: constant value LT.0.0: Load curve ID = (-YC) which defines the transverse compressive strength vs. transverse strain rate (𝜖 ̇𝑏𝑏). YT Transverse tensile strength, 𝑏-axis. GT.0.0: constant value LT.0.0: Load curve ID = (-YT) which defines the transverse tensile strength vs. transverse strain rate (𝜖 ̇𝑏𝑏). VARIABLE DESCRIPTION SL Shear strength, 𝑎𝑏 plane. GT.0.0: constant value LT.0.0: Load curve ID = (-SL) which defines the longitudinal shear strength vs. in-plane shear strain rate (𝜖 ̇𝑎𝑏). XCO Longitudinal compressive strength at inflection point (positive value). GT.0.0: constant value LT.0.0: Load curve ID = (-XCO) which defines the longitudinal compressive strength at inflection point vs. longitudi- nal strain rate (𝜖 ̇𝑎𝑎). XTO Longitudinal tensile strength at inflection point. GT.0.0: constant value LT.0.0: Load curve ID = (-XTO) which defines the longitudinal tensile strength at inflection point vs. longitudinal strain rate (𝜖 ̇𝑎𝑎). FIO Fracture angle in pure transverse compression (in degrees, default = 53.0). SIGY In-plane shear yield stress. GT.0.0: constant value LT.0.0: Load curve ID = (-SIGY) which defines the in-plane shear yield stress vs. in-plane shear strain rate (𝜖 ̇𝑎𝑏). ETAN Tangent modulus for in-plane shear plasticity. GT.0.0: constant value LT.0.0: Load curve ID = (-ETAN) which defines the tangent modulus for in-plane shear plasticity vs. in-plane shear strain rate (𝜖 ̇𝑎𝑏). BETA Hardening parameter for in-plane shear plasticity (0.0 ≤ BETA ≤ 1.0). EQ.0.0: EQ.1.0: Pure kinematic hardening Pure isotropic hardening 0.0 < BETA < 1.0: mixed hardening. PFL *MAT_LAMINATED_FRACTRURE_DAIMLER_CAMANHO DESCRIPTION Percentage of layers which must fail until crashfront is initiated. E.g. |PFL| = 80.0, then 80% of layers must fail until strengths are reduced in neighboring elements. Default: all layers must fail. A single layer fails if 1 in-plane IP fails (PFL > 0) or if 4 in-plane IPs fail (PFL < 0). PUCK Flag for evaluation and post-processing of Puck’s inter-fiber- failure criterion (IFF, see Puck, Kopp and Knops [2002]). EQ.0.0: no evaluation of Puck’s IFF-criterion. EQ.1.0: Puck’s IFF-criterion will be evaluated. SOFT Softening reduction factor for material strength in crashfront elements (default = 1.0). DT Strain rate averaging option. EQ.0.0: Strain rate is evaluated using a running average. LT.0.0: Strain rate is evaluated using average of last 11 time steps. GT.0.0: Strain rate is averaged over the last DT time units. Remarks: The failure surface to limit the elastic domain is assembled by four sub-surfaces, representing different failure mechanisms. They are defined as follows: 1. longitudinal (fiber) tension, 𝜙1+ = 𝜎11 − 𝜐12𝜎22 𝑋𝑇 = 1 2. longitudinal (fiber) compression – (transformation to fracture plane), 𝜙1− = ⟨∣𝜎12 𝑚 ∣ + 𝜇𝐿𝜎22 𝑚 ⟩ 𝑆𝐿 = 1 with 𝜇𝐿 = − 𝑆𝐿 cos(2𝜙0) 𝑌𝐶cos2(𝜙0) 𝜎22 𝑚 = 𝜎11sin2(𝜑𝑐) + 𝜎22cos2(𝜑𝑐) − 2|𝜎12| sin(𝜑𝑐) cos(𝜑𝑐) 𝑚 = (𝜎22 − 𝜎11) sin(𝜑𝑐) cos(𝜑𝑐) + |𝜎12|(cos2(𝜑𝑐) − sin2(𝜑𝑐)) 𝜎12 and 𝜑𝑐 = arctan ⎡1 − √1 − 4 ( ⎢ ⎢ ⎢ ⎢ ⎣ 𝑆𝐿 𝑋𝐶 2 ( 𝑆𝐿 𝑋𝐶 + 𝜇𝐿) 𝑆𝐿 𝑋𝐶 + 𝜇𝐿) ⎤ ⎥ ⎥ ⎥ ⎥ ⎦ 3. transverse (matrix) failure: perpendicular to the laminate mid-plane, 𝜙2+ = ⎧ { { { ⎨ { { { ⎩ √(1 − 𝑔) 𝜎22 𝑌𝑇 +𝑔 ( 𝜎22 𝑌𝑇 ) + ( ) 𝜎12 𝑆𝐿 = 1 𝜎22 ≥ 0 ⟨|𝜎12| + 𝜇𝐿𝜎22⟩ 𝑆𝐿 = 1 𝜎22 < 0 4. transverse (matrix) failure: transverse compression/shear, 𝜙2− = √( 𝜏𝑇 𝑆𝑇 ) + ( 𝜏𝐿 𝑆𝐿 ) = 1 𝑖𝑓 𝜎22 < 0 with 𝜇𝑇 = − tan(2𝜙0) 𝑆𝑇 = 𝑌𝐶 cos(𝜙0) [sin(𝜙0) + 𝜃 = arctan ( −|𝜎12| 𝜎22 sin(𝜙0) ) cos(𝜙0) tan(2𝜙0) ] 𝜏𝑇 = ⟨−𝜎22 cos(𝜙0) [sin(𝜙0) − 𝜇𝑇 cos(𝜙0) cos(𝜃)]⟩ 𝜏𝐿 = ⟨cos(𝜙0) [|𝜎12| + 𝜇𝐿𝜎22 cos(𝜙0) sin(𝜃)]⟩ So long as the stress state is located within the failure surface the model behaves orthotropic elastic. The constitutive law is derived on basis of a proper definition for the ply complementary free energy density 𝐺, whose second derivative with respect to the stress tensor leads to the compliance tensor 𝐇 𝐇 = 𝜕2𝐺 𝜕𝜎 2 = (1 − 𝑑1)𝐸1 𝜐12 𝐸1 − − 𝜐21 𝐸2 (1 − 𝑑2)𝐸2 ⎡ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎣ ⎤ ⎥ ⎥ ⎥ ⎥ ⎥ ⎥ (1 − 𝑑6)𝐺12⎦ , 𝑑1 = 𝑑1+ 𝑑2 = 𝑑2+ 〈𝜎11〉 |𝜎11| 〈𝜎22〉 |𝜎22| + 𝑑1− + 𝑑2− 〈−𝜎11〉 |𝜎11| 〈−𝜎22〉 |𝜎22| Damage evolution: Figure M262-1. Damage evolution law Figure M262-2. In-plane shear behavior Once the stress state reaches the failure criterion a set of scalar damage variables (𝑑1−, 𝑑1+, 𝑑2−, 𝑑2+, 𝑑6) is introduced associated with the different failure mechanisms. A bi-linear (longitudinal direction) and a linear (transverse direction) damage evolution law is utilized to define the development of the damage variables driven by the fracture toughness and a characteristic internal element length to account for objectivity. See Figure M262-1. To account for the characteristic non-linear in-plane shear behavior of laminated fiber- reinforced composites a 1D elasto-plastic formulation with linear hardening is coupled to a linear damage behavior once the maximum allowable stress state for shear failure is reached. See Figure M262-2. More detailed information about this material model can be found in Maimí, Camanho, Mayugo and Dávila [2007]. When failure has occurred in all the composite layers (through-thickness integration points), the element is deleted. Elements which share nodes with the deleted element become “crashfront” elements and can have their strengths reduced by using the SOFT parameter. An earlier initiation of crashfront elements is possible by using the parameter PFL. The number of additional integration point variables written to the LS-DYNA database is input by the *DATABASE_EXTENT_BINARY definition with the variable NEIPS (shells) and NEIPH (solids). These additional variables are tabulated below (i = integration point): Description Value LS-PrePost history variable History Variable 𝜙1+(i) 𝜙1−(i) 𝜙2+(i) 𝜙2−(i) 𝑑1+(i) 𝑑1−(i) 𝑑2(i) 𝑑6(i) fiber tensile mode fiber compressive tensile matrix mode compressive mode damage fiber tension damage compression damage transverse damage in-plane shear matrix fiber dam(i) crashfront fmt_p(i) fmc_p(i) theta_p(i) tensile matrix mod (Puck criteria) compressive mode (Puck criteria) angle of fracture plane (radians, Puck criteria) matrix 0 → 1: elastic 1: failure criterion rea- ched 0: elastic 1: fully damaged -1: element intact 10 - 8: element in crashfront +1: element failed 0 → 1: elastic 1: failure criterion reached 1 2 3 4 5 6 7 8 9 10 11 12 *MAT_TABULATED_JOHNSON_COOK_ORTHO_PLASTICITY This is Material Type 264. This is an orthotropic elastic plastic material law with J3 dependent yield surface. This material considers tensile/compressive asymmetry in the material response, which is important for HCP metals like Titanium. The model is available for solid elements. Card 1 1 Variable MID 2 RO Type A8 F 3 E F 4 PR F 5 CP F 6 TR F 7 8 BETA NUMINT F F Default none none none none none 0.0 1.0 1.0 Card 2 1 2 3 4 5 Variable LCT00R LCT00T LCF LCG LCH Type Default F 0 Card 3 1 F 0 2 F 0 3 F 0 4 Variable LCC00R LCC00T LCS45R LCS45T Type Default F 0 F 0 F 0 F 0 F 0 5 F 0 6 LCI F 0 6 7 8 7 8 SFIEPM NITER AOPT F F 1 100 Card 4 1 2 3 4 5 6 7 8 Variable LCT90R LCT45R LCTTHR LCC90R LCC45R LCCTHR Type Default F 0 Card 5 1 F 0 2 F 0 3 F 0 4 F 0 5 F 0 6 Variable LCT90T LCT45T LCTTHT LCC90T LCC45T LCCTHT F 0 2 YP F 2 V2 F F 0 3 ZP F 3 V3 F F 0 4 A1 F 4 D1 F F 0 5 A2 F 5 D2 F F 0 6 A3 F 6 D3 F 7 8 7 8 MACF F 7 BETA F 8 Type Default Card 6 Variable F 0 1 XP Type F Card 7 Variable 1 V1 Type F VARIABLE MID DESCRIPTION Material identification. A unique number or label not exceeding 8 characters must be specified. RO Mass density. *MAT_TABULATED_JOHNSON_COOK_ORTHO_PLASTICITY DESCRIPTION E Young’s modulus: GT.0.0: constant value is used LT.0.0: temperature dependent Young’s modulus given by load curve ID = -E PR CP TR Poisson’s ratio. Specific heat. Room temperature. BETA Fraction of plastic work converted into heat. NUMINT Number of integration points which must fail before the element is deleted. LCT00R LCT00T LCF LCG LCH LCI EQ.-200: Turns off erosion for solids. Not recommended unless used in conjunction with *CONSTRAINED_- TIED_NODES_FAILURE. Table ID defining for each plastic strain rate value a load curve ID giving the (isothermal) tensile yield stress versus plastic strain for that rate in the 00 degree direction. Table ID defining for each temperature value a load curve ID giving the (quasi-static) tensile yield stress versus plastic strain for that temperature in the 00 degree direction. Load curve ID or Table ID. The load curve ID defines plastic failure strain as a function of triaxiality. The table ID defines for each Lode parameter a load curve ID giving the plastic failure strain versus triaxiality for that Lode parameter. (Table option only for solids and not yet generally supported). Load curve ID defining plastic failure strain as a function of plastic strain rate. Load curve ID defining plastic failure strain as a function of temperature Load curve ID or Table ID. The load curve ID defines plastic failure strain as a function of element size. The table ID defines for each triaxiality a load curve ID giving the plastic failure strain versus element size for that triaxiality. VARIABLE LCC00R LCC00T LCS45R LCS45T DESCRIPTION Table ID. The curves in this table define compressive yield stress as a function of plastic strain. The table ID defines for each plastic strain rate value a load curve ID giving the (isothermal) compressive yield stress versus plastic strain for that rate in the 00 direction. Table ID defining for each temperature value a load curve ID giving the (quasi-static) compressive yield stress versus strain for that temperature. The curves in this table define compressive yield stress as a function of plastic strain in the 00 direction. Table ID. The load curves define shear yield stress in function of plastic strain. The table ID defines for each plastic strain rate value a load curve ID giving the (isothermal) shear yield stress versus plastic strain for that rate in the 45 degree direction. Table ID defining for each temperature value a load curve ID giving the (quasi-static) shear yield stress versus strain for that temperature. The load curves define shear yield stress as a function of plastic strain or effective plastic strain in the 45 degree direction. SFIEPM Scale factor on the initial estimate of the plastic multiplier. NITER Maximum number of iterations for the plasticity algorithm AOPT LCT90R LCT45R LCTTHR LCC90R LCC45R *MAT_TABULATED_JOHNSON_COOK_ORTHO_PLASTICITY DESCRIPTION Material axes option : EQ.0.0: locally orthotropic with material axes determined by element nodes 1, 2, and 4, as with *DEFINE_COORDI- NATE_NODES, and then rotated about the shell ele- ment normal by an angle BETA. EQ.2.0: globally orthotropic with material axes determined by vectors defined below, as with *DEFINE_COORDI- NATE_VECTOR. EQ.3.0: locally orthotropic material axes determined by rotating the material axes about the element normal by an angle, BETA, from a line in the plane of the element defined by the cross product of the vector v with the element normal. LT.0.0: the absolute value of AOPT is a coordinate system ID number (CID on *DEFINE_COORDINATE_NODES, *DEFINE_COORDINATE_SYSTEM or *DEFINE_CO- ORDINATE_VECTOR). Available with the R3 release of Version 971 and later. Table ID defining for each plastic strain rate value a load curve ID giving the (isothermal) tensile yield stress versus plastic strain for that rate in the 90 degree direction. Table ID defining for each plastic strain rate value a load curve ID giving the (isothermal) tensile yield stress versus plastic strain for that rate in the 45 degree direction. Table ID defining for each plastic strain rate value a load curve ID giving the (isothermal) tensile yield stress versus plastic strain for that rate in the thickness degree direction. Table ID defining for each plastic strain rate value a load curve ID giving the (isothermal) compressive yield stress versus plastic strain for that rate in the 90 degree direction. Table ID defining for each plastic strain rate value a load curve ID giving the (isothermal) compressive yield stress versus plastic strain for that rate in the 45 degree direction. VARIABLE LCCTHR LCT90T LCT45T LCTTHT LCC90T LCC45T LCCTHT DESCRIPTION Table ID defining for each plastic strain rate value a load curve ID giving the (isothermal) compressive yield stress versus plastic strain for that rate in the thickness degree direction. Table ID defining for each temperature value a load curve ID giving the (quasistatic) tensile yield stress versus plastic strain for that rate in the 90 degree direction. Table ID defining for each temperature value a load curve ID giving the (quasistatic) tensile yield stress versus plastic strain for that rate in the 45 degree direction. Table ID defining for each temperature value a load curve ID giving the (quasistatic) tensile yield stress versus plastic strain for that rate in the thickness degree direction. Table ID defining for each temperature value a load curve ID giving the (quasistatic) compressive yield stress versus plastic strain for that rate in the 90 degree direction. Table ID defining for each temperature value a load curve ID giving the (quasistatic) compressive yield stress versus plastic strain for that rate in the 45 degree direction. Table ID defining for each temperature value a load curve ID giving the (quasistatic) compressive yield stress versus plastic strain for that rate in the thickness degree direction. A1, A2, A3 Components of vector 𝐚 for AOPT = 2. MACF Material axes change flag for brick elements: EQ.1: No change, default, EQ.2: switch material axes 𝑎 and 𝑏, EQ.3: switch material axes 𝑎 and 𝑐, EQ.4: switch material axes 𝑏 and 𝑐. V1, V2, V3 Components of vector 𝐯 for AOPT = 3. D1, D2, D3 Components of vector 𝐝for AOPT = 2. BETA Material angle in degrees for AOPT = 0 and 3, may be overridden on the element card, see *ELEMENT_SHELL_BETA. *MAT_TABULATED_JOHNSON_COOK_ORTHO_PLASTICITY If IFLAG = 0 the compressive and shear curves are defined as follows: σ𝑐(𝜀𝑝𝑐, 𝜀̇𝑝𝑐), 𝜀𝑝𝑐 = 𝜀𝑐 − σ𝑠(𝛾𝑝𝑠, 𝛾̇𝑝𝑠), 𝛾𝑝𝑠 = 𝛾𝑠 − 𝜎𝑐 𝜎𝑠 , 𝜀̇𝑝𝑐 = , 𝛾̇𝑝𝑠 = 𝜕𝜀𝑝𝑐 𝜕𝑡 𝜕𝛾𝑝𝑠 𝜕𝑡 and two new history variables (#15 plastic strain in compression and #16 plastic strain in shear) are stored in addition to those history variables already stored in MAT_224. If IFLAG = 1 the compressive and shear curves are defined as follows: σ𝑐(𝜆̇, 𝜆), 𝜎𝑠(𝜆̇, 𝜆), 𝑊𝑝̇ = 𝜎eff𝜆̇ History variables may be post-processed through additional variables. The number of additional variables for solids written to the d3plot and d3thdt databases is input by the optional *DATABASE_EXTENT_BINARY card as variable NEIPH. The relevant additional variables of this material model are tabulated below: LS-PrePost history variable # 5 6 7 8 9 10 11 12 13 14 15 16 Solid elements plastic strain rate Compressive plastic strain Shear plastic strain plastic failure strain triaxiality Lode parameter plastic work ratio of plastic strain to plastic failure strain element size temperature plastic strain in compression plastic strain in shear *MAT_TISSUE_DISPERSED This is Material Type 266. This material is an invariant formulation for dispersed orthotropy in soft tissues, e.g., heart valves, arterial walls or other tissues where one or two collagen fibers are used. The passive contribution is composed of an isotropic and two anisotropic parts. The isotropic part is a simple neo-Hookean model. The first anisotropic part is passive, with two collagen fibers to choose from: (1) a simple exponential model and (2) a more advanced crimped fiber model from Freed et al. [2005]. The second anisotropic part is active described in Guccione et al. [1993] and is used for active contraction. Card 1 1 Variable MID Type I Card 2 1 2 RO F 2 Variable FID ORTH Type I Card 3 1 I 2 3 F F 3 C1 F 3 4 5 6 7 8 SIGMA MU KAPPA ACT INIT F F 4 C2 F 4 5 C3 F 5 F 6 I 7 THETA NHMOD F 6 F 7 I 8 8 Variable ACT1 ACT2 ACT3 ACT4 ACT5 ACT6 ACT7 ACT8 Type F Card 4 1 F 2 F 3 F 4 F 5 F 6 F 7 F 8 Variable ACT9 ACT10 Type F Card 5 1 2 Variable AOPT BETA Type I F Card 6 Variable 1 V1 Type F 2 V2 F 3 XP F 3 V3 F 4 YP F 4 D1 F 5 ZP F 5 D2 F 6 A1 F 6 D3 F 7 A2 F 7 8 A3 F 8 VARIABLE DESCRIPTION MID Material identification. A unique number must be specified. RO F SIGMA Mass density. Fiber dispersion parameter governs the extent to which the fiber dispersion extends to the third dimension. F = 0 and F = 1 apply to 2D splay with the normal to the membrane being in the 𝛽 and the 𝛾-directions, respectively . F = 0.5 applies to 3D splay with transverse isotropy. Splay will be orthotropic wheneverF ≠ 0.5. This parameter is ignored if INIT = 1. The parameter SIGMA governs the extent of dispersion, such that as SIGMA goes to zero, the material symmetry reduces to pure transverse isotropy. Conversely, as SIGMA becomes large, the This material symmetry becomes isotropic in the plane. parameter is ignored if INIT = 1. MU MU is the isotropic shear modulus that models elastin. MU should be chosen such that the following relation is satisfied: 0.5 (3KAPPA − 2MU) (3KAPPA + MU) ⁄ < 0.5. Instability can occur for implicit simulations if this quotient is close to 0.5. A modest approach is a quotient between 0.495 and 0.497. KAPPA Bulk modulus for the hydrostatic pressure. ACT INIT FID ORTH *MAT_TISSUE_DISPERSED DESCRIPTION ACT = 1 indicates that an active model will be used that acts in the mean fiber-direction. The active model, like the passive model, will be dispersed by SIGMA and F, or if INIT = 1, with the *INITIAL_FIELD_SOLID keyword. INIT = 1 indicates that the anisotropy eigenvalues will be given by *INITIAL_FIELD_SOLID variables in the global coordinate system . The passive fiber model number. There are two passive models available: FID = 1 or FID = 2. They are described in Remark 2. ORTH specifies the number (1 or 2) of fibers used. When ORTH = 2 two fiber families are used and arranges symmetrically THETA degrees from the mean fiber direction and lying in the tissue plane. C1-C3 Passive fiber model parameters. THETA The angle between the mean fiber direction and the fiber families. The parameter is active only if ORTH = 2 and is particularly important in vascular tissues (e.g. arteries) NHMOD Neo-Hooke model flag ACT1 - ACT10 AOPT EQ.0.0: original implementation (modified Neo-Hooke) EQ.1.0: standard Neo-Hooke model (as in umat45 of dyn21.f) Active fiber model parameters. Note that ACT10 is an input for a time dependent load curve that overrides some of the ACTx values. See section 2 below. Material axes option : EQ.0.0: locally orthotropic with material axes determined by element nodes 1, 2, and 4, as with *DEFINE_COORDI- NATE_NODES. EQ.2.0: globally orthotropic with material axes determined by vectors defined below, as with *DEFINE_COORDI- NATE_VECTOR. EQ.3.0: locally orthotropic material axes determined by rotating the material axes about the element normal by an angle, BETA, from a line in the plane of the element 2 𝛽 3 𝛾 𝛼 Figure M266-1. The plot on the left relates the global coordinates (1, 2, 3) to the local coordinates (𝛼, 𝛽, 𝛾), selected so the mean fiber direction in the reference configuration is align with the 𝛼–axis. The plots on the right show how the unit vector for a specific fiber within the fiber distribution of a 3D tissue is oriented with respect to the mean fiber direction via angles 𝜃 and 𝜙. VARIABLE DESCRIPTION defined by the cross product of the vector v with the element normal. LT.0.0: the absolute value of AOPT is a coordinate system ID number (CID on *DEFINE_COORDINATE_NODES, *DEFINE_COORDINATE_SYSTEM or *DEFINE_CO- ORDINATE_VECTOR). Available with the R3 release of Version 971 and later. BETA P1 - P3 Material angle in degrees for AOPT = 3, may be overridden on the element card *ELEMANT_SOLID_ORTHO. P1, P2 and P3 define the coordinates of point P for AOPT = 1 and AOPT = 4. A1 - A3 A1, A2 and A3 define the components of vector A for AOPT = 2. D1 - D3 D1, D2 and D3 define components of vector D for AOPT = 2. V1 - V3 V1, V2 and V3 define components of vector V for AOPT = 3 and AOPT = 4. Details of the passive model can be found in Freed et al. (2005) and Einstein et al. (2005). The stress in the reference configuration consists of a deviatoric matrix term, a hydrostatic pressure term, and either one (ORTHO = 1) or two (ORTH = 2) fiber terms: 𝐒 = 𝜅𝐽(𝐽 − 1)𝐂−1 + 𝜇𝐽−2 3⁄ 𝐃𝐄𝐕 [ (𝐈 − 𝐂̅−2)] + 𝐽−2 3⁄ ∑[𝜎𝑖(𝜆𝑖) + 𝜀𝑖(𝜆𝑖)]𝐃𝐄𝐕[𝐊𝑖] 𝑖=1 where S is the second Piola-Kirchhoff stress tensor, J is the Jacobian of the deformation gradient, 𝜅 is the bulk modulus, 𝜎𝑖 is the passive fiber stress model used, and 𝜀𝑖 is the corresponding active fiber model used. The operator DEV is the deviatoric projection: 𝐃𝐄𝐕[•] = (•) − tr[(•)𝐂]𝐂−1 where C is the right Cauchy-Green deformation tensor. The dispersed fourth invariant 𝜆 = √tr[𝐊𝐂̅], where 𝐂̅is the isochoric part of the Cauchy-Green deformation. Note that 𝜆 is not a stretch in the classical way, since K embeds the concept of dispersion. K is called the dispersion tensor or anisotropy tensor and is given in global coordinates. The passive and active fiber models are defined in the fiber coordinate system. In effect the dispersion tensor rotates and weights these one dimensional models, such that they are both three-dimensional and in the Cartesian framework. In the case where, the splay parameters SIGMA and F are specified, K is given by: 𝐊𝑖 = 𝐐𝑖 ⎡1 + 𝑒−2SIGMA2 ⎢⎢⎢ ⎣ F(1 − 𝑒−2SIGMA2 ) 0 (1 − F)(1 − 𝑒−2SIGMA2 𝑇 𝐐𝑖 ⎤ ⎥⎥⎥ )⎦ where Q is the transformation tensor that rotates from the local to the global Cartesian system. In the case when INIT = 1, the dispersion tensor is given by 𝐊𝑖 = 𝐐𝑖 𝜒𝑖 ⎜⎜⎜⎜⎛ ⎝ 𝜒𝑖 ⎟⎟⎟⎟⎞ 3⎠ 𝜒𝑖 𝑇 𝐐𝑖 where the 𝜒:s are given on the *INITIAL_FIELD_SOLID card. For the values to be 3 = 1. It is the responsibility of the user to assure that physically meaningful 𝜒𝑖 this condition is met, no internal checking for this is done. These values typically come from diffusion tensor data taken from the myocardium. 2 + 𝜒𝑖 1 + 𝜒𝑖 Remarks: 1. Passive fiber models. Currently there are two models available. a) If FID = 1 a crimped fiber model is used. It is solely developed for colla- gen fibers. Given 𝐻0 and 𝑅0 compute: 𝐿0 = √(2𝜋)2 + (𝐻0)2, Λ = 𝐿0 𝐻0 and 2.5 1.5 0.5 0.98 Crimped Model Exp Model 1.02 1.04 1.06 1.08 1.1 1.12 1.14 1.16 Stretch Figure M266-2. both the Crimped and the Exponential fiber models visualized. Here ۓ = 1.1 is the transition point in the crimped model. 𝐸𝑓 𝐻0 . 𝐸𝑠 = 𝐻0 + (1 + 37 6𝜋2 + 2 Now if the fiber stretches 𝜆 < Λ the fiber stress is given by: 𝐿0 𝜋2) (𝐿0 − 𝐻0) 𝜉 = where 𝜎 = 𝜉 𝐸𝑠(𝜆 − 1) 6𝜋2(Λ2 + (4𝜋2 − 1)𝜆2)𝜆 Λ(3𝐻0 2(Λ2 − 𝜆2)(3Λ2 + (8𝜋2 − 3)𝜆2) + 8𝜋2(10Λ2 + (3𝜋2 − 10)𝜆2)) and if 𝜆 > Λ the fiber stress equals: 𝜎 = 𝐸𝑠(𝜆 − 1) + 𝐸𝑓 (𝜆 − Λ). In Figure M266-1 the fiber stress is rendered with 𝐻0 = 27.5, 𝑅0 = 2 and the transition point becomes Λ = 1.1. b) The second fiber model available (FID = 2) is a simpler but more useful model for the general fiber reinforced rubber. The fiber stress is simply given by: 𝜎 = 𝐶1 [𝑒 𝐶2 (𝜆2−1) − 1]. The difference between the two fiber models is given in Figure M266-2. The active model for myofibers (ACT = 1) is defined in Guccione et al. (1993) and is given by: 𝜎 = 𝑇max where 𝐶𝑎0 2 + 𝐸𝐶𝑎50 𝐶𝑎0 2 𝐶(𝑡) 2 = 𝐸𝐶𝑎50 (𝐶𝑎0)max √𝑒𝐵(𝑙𝑟√2(𝜆−1)+1−𝑙0)−1 and 𝐵 is a constant, (𝐶𝑎0)max is the maximum peak intracellular calcium con- centration, 𝑙0 is the sarcomere length at which no active tension develops and 𝑙𝑟 is the stress free sarcomere length. The function 𝐶(𝑡) is defined in one of two ways. First it can be given as: where 𝐶(𝑡) = (1 − cos𝜔(𝑡)) 𝜔 = 𝑡0 𝑡 − 𝑡0 + 𝑡𝑟 𝑡𝑟 ⎧ { { { ⎨ { { { ⎩ 0 ≤ 𝑡 < 𝑡0 𝑡0 ≤ 𝑡 < 𝑡0 + 𝑡𝑟 𝑡0 + 𝑡𝑟 ≤ 𝑡 and 𝑡𝑟 = 𝑚𝑙𝑅𝜆 + 𝑏. Secondly, it can also be given as a load curve. If a load curve should be used its index must be given in ACT10. Note that all variables that correspond to ω are neglected if a load curve is used. The active parameters on Card 3 and 4 are interpreted as: ACT1 ACT2 ACT3 ACT4 ACT5 ACT6 ACT7 ACT8 ACT9 ACT10 𝑇max 𝐶𝑎0 (𝐶𝑎0)max 𝑙0 𝑡0 𝑙𝑅 LCID References: 1. Freed AD., Einstein DR. and Vesely I., Invariant formulation for dispersed transverse isotropy in aortic heart valves – An efficient means for modeling fiber splay, Biomechan model Mechanobiol, 4, 100-117, 2005. 2. Guccione JM., Waldman LK., McCulloch AD., Mechanics of Active Contraction in Cardiac Muscle: Part II – Cylindrical Models of the Systolic Left Ventricle, J. Bio Mech, 115, 82-90, 1993. *MAT_267 This is Material Type 267. This is an advanced rubber-like model that is tailored for glassy polymers and similar materials. It is based on Arruda´s eight chain model but enhanced with non elastic properties. Card 1 1 Variable MID Type I 2 RO F 3 K F 4 MU F Default none none 0.0 0.0 Card 2 1 Variable YLD0 Type F 2 FP F 3 GP F 4 HP F 5 N I 0 5 LP F 6 7 8 MULL VISPL VISEL I 0 6 MP F I 0 7 NP F I 0 8 PMU F Default 0.0 0.0 0.0 0.0 0.0 0.0 0.0 0.0 Card 3 1 Variable M1 2 M2 3 M3 4 M4 5 6 7 8 M5 TIME VCON Type F F F F F F F Default See MULL See MULL See MULL See MULL See MULL 0.0 9.0 Variable 1 Q1 Type F *MAT_EIGHT_CHAIN_RUBBER 2 B1 F 3 Q2 F 4 B2 F 5 Q3 F 6 B3 F 7 Q4 F 8 B4 F Default 0.0 0.0 0.0 0.0 0.0 0.0 0.0 0.0 Card 5 Variable 1 K1 Type F 2 S1 F 3 K2 F 4 S2 F 5 K3 F 6 S3 F 7 8 Default 0.0 0.0 0.0 0.0 0.0 0.0 Card 6 1 2 Variable AOPT MACF Type F F 3 XP F 4 YP F 5 ZP F 6 A1 F 7 A2 F 8 A3 F Default 0.0 0.0 0.0 0.0 0.0 0.0 0.0 .0.0 Card 7 Variable 1 V1 Type F 2 V2 F 3 V3 F 4 D1 F 5 D2 F 6 D3 F 7 8 THETA F Default 0.0 0.0 0.0 0.0 0.0 0.0 0.0 Card 8-14 1 2 3 4 5 6 7 8 Variable TAUi BETAi Type F F Default 0.0 0.0 VARIABLE DESCRIPTION MID Material identification. A unique number must be specified RO K MU MULL Mass density. Bulk modulus. To get almost incompressible behavior set this to one or two orders of magnitude higher than MU. Note that the poisons ratio should be kept at a realistic value. 𝜐 = 3𝐾 − 2𝑀𝑈 2(3𝐾 + 𝑀𝑈) . Shear modulus. MU is the product of the number of molecular chains per unit volume (n), Boltzmann’s constant (k) and the absolute temperature (T). Thus MU = nkT. Parameter describing which softening algorithm that shall be used. EQ.1: Strain based Mullins effect from Qi and Boyce, see theory section below for details M1 = A (Qi recommends 3.5) M2 = B (Qi recommends 18.0) M3 = Z (Qi recommends 0.7) M4 = vs (between 0 and 1 and less than vss) M5 = vss (between 0 and 1 and greater than vs) EQ.2: Energy based Mullins, a modified version of Roxburgh and Ogden model. M1 > 0, M2 > 0 and M3 > 0 must be set. See Theory section for details. VISPL *MAT_EIGHT_CHAIN_RUBBER DESCRIPTION Parameter describing which viscoplastic formulation that should be used, see the theory section for details. EQ.0: No viscoplasticity. EQ.1: 2 parameters standard model, K1 and S1 must be set. EQ.2: 6 parameters G’Sells model, K1,K2,K3,S1,S2 and S3 must be set. EQ.3: 4 parameters Strain hardening model, K1,K2,S1,S2 must be set. VISEL Option for viscoelastic behavior, see the theory section for details. EQ.0: No viscoelasticity. EQ.1: Free energy formulation based on Holzapfel and Ogden. EQ.2: Formulation based on stiffness ratios from Simo et al. YLD0 Initial yield stress. EQ.0.0: No plasticity GT.0.0: Initial yield stress: seperataly. Hardening is defined LT.0.0: -YLD0 is taken as the load curve ID for the yield stress versus effective plastic strain. FP-NP Parameters for Hill’s general yield surface. For von mises yield criteria set FP = GP = HP = 0.5 and LP = MP = NP = 1.5. PMU Kinematic hardening parameter. It is usually equal to MU. M1 - M5 Mullins parameters MULL.EQ.1: M1 - M5 are used MULL.EQ.2: M1 - M3 are used. TIME VCON A time filter that is used to smoothen out the time derivate of the strain invariant over a TIME interval. Default is no smoothening but a value 100*TIMESTEP is recommended. A material constant for the volumetric part of the strain energy. Default 9.0 but any value can be used to tailor the volumetric response. For example -2. VARIABLE DESCRIPTION Q1 - B4 Voce hardening parameters K1 - S3 Viscoplastic parameters. VISPL.EQ.1: K1 and S1 are used. VISPL.EQ.2: K1, S1, K2, S2, K3 and S3 are used. VISPL.EQ.3: K1, S1 and K2 are used. AOPT Material axes option for a more complete description. EQ.0.0: Locally orthotropic with material axes defined by element nodes 1, 2 and 4. EQ.1.0: Locally orthotropic with material axes determined by a point in space and the global location of the element center; this is the a-direction. EQ.2.0: Globally orthotropic with material axes determined by vectors defined below. EQ.3.0: Locally orthotropic material axes determined by rotating the material axes about the element normal by and angle THETA. The angle is defined from the line in the plane that is defined by the cross product of the vector v with the element normal. The plane of a solid is defined as the midsurface between the inner surface and the outer surface defined by the first 4 nodes and last 4 nodes. EQ.4.0: Locally orthotropic in cylindrical coordinate system with the material axes determined by a vector v and an originating point P. MACF Material axes change flag EQ.1.0: No change (default) EQ.2.0: Switch axes a and b EQ.3.0: Switch axes a and c EQ.4.0: Switch axes b and c XP, YP, ZP Define coordinates for point P for AOPT = 1 and 4 A1, A2, A3 Define components of vector a for AOPT = 2. *MAT_EIGHT_CHAIN_RUBBER DESCRIPTION D1, D2, D3 Define components of vector d for AOPT = 2 V1, V2, V3 Define components of vector v for AOPT = 3 and 4 TAUi Relaxation time. A maximum of 6 values can be used. BETAi / GAMMAi VISEL.EQ.1: Dissipating energy factors. VISEL.EQ.2: Gamma factors Basic theory: This model is based on the work done by Arruda and Boyce [1993], in particular Arruda’s thesis [1992]. The eight chain rubber model is based on hyper elasticity and it is formulated by using strain invariants. The strain softening is taken from work done by Qi and Boyce [2004], where the strain energy used is defined as Ψ = 𝑣𝑠𝜇 [√𝑁Λ𝑐𝛽 + 𝑁ln ( sinh𝛽 )] + Ψ2 = Ψ1 + Ψ2, where the amplified chain stretch is given by Λ𝑐 = √𝑋(𝜆̅̅̅̅2 − 1) + 1and 𝛽 = 𝐿−1 ⎜⎛ Λ𝑐 ⎟⎞, √𝑁⎠ ⎝ where 𝜆̅̅̅̅2 = 𝐼1 3⁄ , 𝜇 is the initial modulus of the soft domain, N is the number of rigid links between crosslinks of the soft domain region. 𝑋 = 1 + 𝐴(1 − 𝑣𝑠) + 𝐵(1 − 𝑣𝑠)2, is a general polynomial describing the interaction between the soft and the hard phases (Qi and Boyce [2004] and Tobin and Mullins [1957]). The compressible behavior is described by the strain energy. Ψ2 = 𝜈con (𝜈conln𝐽 + 𝐽𝜈con − 1) Where J is the determinant of the elastic deformation gradient Fe. The Cauchy stress is then computed as: 𝝈 = 𝐅𝑒 ∂Ψ ∂𝐂𝑒 𝑇 = 𝐅𝑒 𝐅𝑒(𝐒𝟏 + 𝐒𝟐)𝐅𝑒 𝑇 = 𝑣𝑠𝑋𝜇 3𝐽 √𝑁 Λ𝑐 𝐿−1 ⎜⎛ Λ𝑐 √𝑁⎠ ⎝ ⎟⎞ (𝐁𝑒 − 𝐼1𝐈) + 2𝐾 𝐽𝑣con (1 − 𝐽𝑣con ) where 𝐒𝟏 and 𝐒𝟐 are second Piola-Kirchhoff stresses based on Ψ1 and Ψ2 respectively. Mullins effect: Two models for the Mullins effect are implemented. 1. MULL = 1 The strain softening is developed by the evolution law taken from Boyce 2004: 𝑣̇𝑠 = 𝑍(𝑣𝑠𝑠 − 𝑣𝑠) √𝑁 − 1 (√𝑁 − Λ𝑐 max) 2 Λ̇ 𝑐 max, where Z is a parameter that characterizes the evolution in 𝑣𝑠 with increasing Λ̇ 𝑐 maxis the maximum of Λ𝑐 from the past: max. The parameter 𝑣𝑠𝑠 is the saturation value of 𝑣𝑠. Note that Λ̇ 𝑐 Λ̇ 𝑐 max = { Λ𝑐 < Λ𝑐 Λ̇ 𝑐 Λ𝑐 > Λ𝑐 The structure now evolves with the deformation. The dissipation inequality requires that the evolution of the structure is irreversible𝑣̇𝑠 ≥ 0. See Qi and Boyce [2004]. max max. 2. MULL = 3 The energy driven model based on Ogden and Roxburgh. When activated the strain eergy is automatically transformed to a standard eight chain model. That is, the variables Z, vs and X is automatically set to 0, 1 and 1 respectively. The stress is multiplicative split of the true stress and the softening factor η. 𝜎̅̅̅̅̅ = 𝜂𝜎, 𝜂 = 1 − 𝑀1 Viscoelasticity: 1. VISEL = 1 erf ( Ψ1 max − Ψ1 𝑀3 − 𝑀2Ψ1 max). The viscoelasticity is based on work dine by Holzapfel (2004) 𝐐̇ 𝛼 + 𝐐𝛼 𝜏𝛼 = 2𝛽𝛼 𝑑𝑡 ∂Ψ1 ∂𝐂𝑒 = 𝛽𝛼𝐒̇𝟏 where 𝛼 is the number of viscoelastic terms (0, 1,…, 6). 2. VISEL = 2 With this option the evolution is based on work done by Simo and Hughes (2000). 𝐐̇ 𝛼 + 𝐐𝛼 𝜏𝛼 = 2 𝛾𝑎 𝜏𝑎 𝑑𝑡 ∂Ψ1 ∂𝐂𝑒 = 𝛾𝑎 𝜏𝑎 𝐒𝟏 The the number of Prony terms is restricted to maximum 6 and τ > 0, γ > 0. The Cauchy stress is obtained by a push forward operation on the total second Piola-Kirchhoff stress. σ = 𝐅𝑒𝐒𝐅𝑒 𝑇. Viscoplasticity: The plasticity is based on the general Hills’ yield surface 2 = 𝐹(𝜎22 − 𝜎33)2 + 𝐺(𝜎33 − 𝜎11)2 + 𝐻(𝜎11 − 𝜎22)2 + 2𝐿𝜎12 𝜎eff 2 + 2𝑀𝜎23 2 2 + 2𝑁𝜎13 and the hardening is either based on a load curve ID (-YLD0) or an extended Voce hardening 𝜎yld = 𝜎yld0 + 𝑄1(1 − 𝑒𝐵1𝜀̅) + 𝑄2(1 − 𝑒𝐵2𝜀̅) + 𝑄3(1 − 𝑒𝐵3𝜀̅) + 𝑄4(1 − 𝑒𝐵4𝜀̅). The yield criterion is written 𝑓 = 𝜎eff − 𝜎yld ≤ 0. Adding the viscoplastic phenomena, we simply add one evolution equation for the effective plastic strain rate. Three different formulations is available. 1. VISPL = 1 ̇vp = ( 𝜀̅ 𝑆1 ) . 𝐾1 where K1 and S1 are viscoplastic material parameters. 2. VISPL = 2 𝜀̇vp = ⎡ ⎢⎢ ⎣ 𝐾3 𝐾1(1 − 𝑒−𝑆1(𝜀vp+𝐾2))𝑒𝑆2𝜀𝑣𝑝 𝑆3 ⎤ ⎥⎥ ⎦ Where K1, K2, K3, S1, S2 and S3 are viscoplastic parameters 3. VISPL = 3 𝜀̇vp = ( 𝐾1 𝑆1 ) (𝜀vp + 𝐾2) 𝑆2 Where K1, K2, S1 and S2 are viscoplastic parameters. Kinematic hardening: The back stress is calculated similar to the Cauchy stress above but without the softening factors: β = 𝜇𝑝 3𝐽 √𝑁 Λ𝑐 𝐿−1 ⎜⎛ Λ𝑐 √𝑁⎠ ⎝ ⎟⎞ (𝐈 − 𝐼𝑝𝐂𝑝 −1) 𝜇𝑝is a hardening material parameter (PMU). The total Piola-Kirchhoff stress is now given by 𝐒∗ = 𝐒 − β and the total stress is given by a standard push forward operation with the elastic deformation gradient. Remarks: 1. The parameter PMU is usually taken the same as MU. 2. For the case of a dilute solution the Mullins parameter A should be equal to 3.5. See Qi and Boyce [2004]. 3. For a system with well dispersed particles B should somewhere around 18. See Qi and Boyce [2004]. References: Qi HJ., Boyce MC., Constitutive model for stretch-induced softening of stress-stretch behavior of elastomeric materials, Journal of the Mechanics and Physics of Solids, 52, 2187-2205, 2004. Arrude EM., Characterization of the strain hardening response of amorphous polymers, PhD Thesis, MIT, 1992. Mullins L., Tobin NR., Theoretical model for the elastic behavior of filler reinforced vulcanized rubber, Rubber Chem. Technol., 30, 555-571, 1957. Ogden RW. Roxburgh DG., A pseudo-elastic model for the Mullins effect in Filled rubber., Proc. R. Soc. Lond. A., 455, 2861-2877, 1999. Simo JC., Hughes TJR., Computational Inelasticity, Springer, New York, 2000. Holzapfel GA., Nonlinear Solid Mechanics, Wiley, New-York, 2000. *MAT_BERGSTROM_BOYCE_RUBBER This is material type 269. This is a rubber model based on the Arruda and Boyce (1993) chain model accompanied with a viscoelastic contribution according to Bergström and Boyce (1998). The viscoelastic treatment is based on the physical response of a single entangled chain in an embedded polymer gel matrix and the implementation is based on Dal and Kaliske (2009). This model is only available for solid elements. Card 1 1 Variable MID 2 RO Type A8 F 3 K F 4 G F 5 GV F 6 N F 7 NV F 8 Default none none none none none none none Card 2 Variable Type 1 C F 2 M F 3 4 5 6 7 8 GAM0 TAUH F F Default none none none none VARIABLE DESCRIPTION MID Material identification. A unique number or label not exceeding 8 characters must be specified. RO Mass density. K G GV N Elastic bulk modulus Elastic shear modulus Viscoelastic shear modulus Elastic segment number VARIABLE DESCRIPTION NV Viscoelastic segment number C M Inelastic strain exponent, should be less than zero Inelastic stress exponent TAUH Reference Kirchhoff stress Remarks: The deviatoric Kirchhoff stress for this model is the sum of an elastic and viscoelastic part according to The elastic part is governed by the Arruda-Boyce strain energy potential resulting in the following expression (after a Pade approximation of the Langevin function) τ̅̅̅̅̅ = τ𝑒 + τ𝑣 τ𝑒 = 3 − 𝜆𝑟 1 − 𝜆𝑟 2 (𝐛̅ − 𝑇𝑟(𝐛̅ ) 𝐈) Here G is the elastic shear modulus, is the unimodular left Cauchy-Green tensor, and 𝐛̅ = 𝐽−2/3𝐅𝐅𝑇 𝐽 = det 𝐅 2 = 𝜆𝑟 𝑇𝑟(𝐛̅ ) 3𝑁 is the relative network stretch. The viscoelastic stress is based on a multiplicative split of the unimodular deformation gradient into unimodular elastic and inelastic parts, respectively, and we define 𝐽−1/3𝐅 = 𝐅𝑒𝐅𝑖 𝑇 𝐛𝑒 = 𝐅𝑒𝐅𝑒 to be the elastic left Cauchy-Green tensor. The viscoelastic stress is given as where τ𝑣 = 𝐺𝑣 3 − 𝜆𝑣 2 (𝐛𝑒 − 1 − 𝜆𝑣 𝑇𝑟(𝐛𝑒) 𝐈) 2 = 𝜆𝑣 𝑇𝑟(𝐛𝑒) 3𝑁𝑣 is the relative network stretch for the viscoelastic part. The evolution of the elastic left Cauchy-Green tensor can be written where the inelastic rate-of-deformation tensor is given as 𝐛̇ 𝑒 = 𝐋̅ 𝐛𝑒 + 𝐛𝑒𝐋̅ 𝑇 − 2𝐃𝑖𝐛𝑒 and 𝐃𝑖 = 𝛾̇0(𝜆𝑖 − 0.999)𝑐 ⎜⎛∥τ𝑣∥ ⎟⎞ 𝜏̂√2⎠ ⎝ 𝑚 τ𝑣 ∥τ𝑣∥ 𝐋̅ = 𝐋 − 𝑇𝑟(𝐋) 𝐈 is the deviatoric velocity gradient. The stretch of a single chain relaxing in a polymer is linked to the inelastic right Cauchy-Green tensor as 2 = 𝜆𝑖 𝑇𝐅𝑖) 𝑇𝑟(𝐅𝑖 ≥ 1, and this stretch is available as the plastic strain variable in the post processing of this material. The volumetric part is elastic and governed by the bulk modulus, the pressure for this model is given as 𝑝 = 𝐾(𝐽−1 − 1). *MAT_270 This is material type 270. This is a thermo-elastic-plastic model with kinematic hardening that allows for material creation as well as annealing triggered by temperature. The acronym CWM stands for Computational Welding Mechanics, Lindström (2013, 2015), and the model is intended to be used for simulating multistage weld processes. This model is available for solid and shell elements. Card 1 1 Variable MID 2 RO 3 4 5 6 7 8 LCEM LCPR LCSY LCHR LCAT BETA Type A8 F F F F F F F Default none none none none none none none None Card 2 1 2 3 4 5 6 7 8 Variable TASTART TAEND TLSTART TLEND EGHOST PGHOST AGHOST Type F F F F F F F Default none none none none none none none Optional Phase Change Card. Card 3 1 2 3 4 5 6 7 8 Variable T2PHASE T1PHASE Type F F Default optional optional VARIABLE MID DESCRIPTION Material identification. A unique number or label not exceeding 8 characters must be specified. RO Material density LCEM Load curve for Young’s modulus as function of temperature LCPR LCSY LCHR LCAT Load curve for Poisson’s ratio as function of temperature Load curve or table for yield stress. GT.0: Yield stress is a load curve as function of temperature. LT.0: |LCSY| is a table of yield curves for different tempera- tures. Each yield curve is a function of plastic strain. Load curve for hardening modulus as function of temperature. LCHR is not used for LCSY.LT.0. Hardening modulus is then calculated from yield curve slope. Load curve (or table) for thermal expansion coefficient as function of temperature (and maximum temperature up to current time). In the case of a table, load curves are listed according to their maximum temperature. BETA Fraction isotropic hardening between 0 and 1 EQ.0: Kinematic hardening EQ.1: Isotropic hardening TASTART Annealing temperature start TAEND Annealing temperature end TLSTART Birth temperature start TLEND Birth temperature end EGHOST Young’s modulus for ghost (quiet) material PGHOST Poisson’s ratio for ghost (quiet) material AGHOST Thermal expansion coefficient for ghost (quiet) material T2PHASE Temperature at which phase change commences T1PHASE Temperature at which phase change ends *MAT_270 This material is initially in a quiet state, sometimes referred to as a ghost material. In this state the material has the thermo-elastic properties defined by the quiet Young’s modulus, quiet Poisson’s ratio and quiet thermal expansion coefficient. These should represent void, i.e., the Young’s modulus should be small enough to not influence the surroundings but large enough to avoid numerical problems. A quiet material stress should never reach the yield point. When the temperature reaches the birth temperature, a history variable representing the indicator of the welding material is incremented. This variable follows 𝛾(𝑡) = min (1, max [0, 𝑇max − 𝑇𝑙 end − 𝑇𝑙 𝑇𝑙 𝑇(𝑠). This parameter is available as history variable 9 in the output ]) start start where 𝑇max = max 𝑠≤𝑡 database. The effective thermo-elastic material properties are interpolated as 𝐸 = 𝐸(𝑇)𝛾 + 𝐸quiet(1 − 𝛾) 𝜈 = 𝜈(𝑇)𝛾 + 𝜈quiet(1 − 𝛾) 𝛼 = 𝛼(𝑇, 𝑇max)𝛾 + 𝛼quiet(1 − 𝛾) where 𝐸, 𝜈, and 𝛼 are the Young’s modulus, Poisson’s ratio and thermal expansion coefficient, respectively. Here, the thermal expansion coefficient is either a temperature dependent curve, or a collection of temperature dependent curves, ordered in a table according to maximum temperature 𝑇max. The stress update then follows a classical isotropic associative thermo-elastic-plastic approach with kinematic hardening that is summarized in the following. The explicit temperature dependence is sometimes dropped for the sake of clarity. The stress evolution is given as where 𝐂 is the effective elastic constitutive tensor and σ̇ = 𝐂(ε̇ − ε̇𝑝 − ε̇𝑇) ε̇𝑇 = 𝛼𝑇̇𝐈 ε̇𝑝 = 𝜀̇𝑝 𝐬 − κ 𝜎̅̅̅̅̅ are the thermal and plastic strain rates, respectively. The latter expression includes the deviatoric stress the back stress κ and the effective stress 𝐬 = 𝛔 − Tr(𝛔)𝐈, 𝜎̅̅̅̅̅ = √ (𝐬 − κ): (𝐬 − κ) that are involved in the plastic equations. To this end, the effective yield stress is given as 𝜎𝑌 = 𝜎𝑌(𝑇) + 𝛽𝐻(𝑇)𝜀𝑝 and plastic strains evolve when the effective stress exceeds this value. The back stress evolves as κ̇ = (1 − 𝛽)𝐻(𝑇)𝜀̇𝑝 𝐬 − κ 𝜎̅̅̅̅̅ where 𝜀̇𝑝 is the rate of effective plastic strain that follows from consistency equations. When the temperature reaches the start annealing temperature, the material starts assuming its virgin properties. Beyond the start annealing temperature it behaves as an ideal elastic-plastic material but with no evolution of plastic strains. The resetting of effective plastic properties in the annealing temperature interval is done by modifying the effective plastic strain and back stress before the stress update as 𝑛+1 = 𝜀𝑝 𝜀𝑝 𝑛max [0, min (1, κ𝑛+1 = κ𝑛max [0, min (1, 𝑇𝑎 end 𝑇 − 𝑇𝑎 start − 𝑇𝑎 end 𝑇 − 𝑇𝑎 start − 𝑇𝑎 𝑇𝑎 )] end )] end The optional Card 3 is used to set history variable 11, which is the average temperature rate by which the temperature has gone from T2PHASE to T1PHASE. To fringe this variable the range should be set to positive values since it is during the simulation temporarily used to store the time when the material has reached temperature T2PHASE and is then stored as a negative value. A strictly positive value means that the material has reached temperature T2PHASE and gone down to T1PHASE and the history variable is (T2PHASE − T1PHASE) (T1 − T2) , where T2 is the time when temperature T2PHASE is reached and T1 is the time when temperature T1PHASE is reached. Note that T2PHASE > T1PHASE and T1 > T2. A value of zero means that the element has not yet reached temperature T2PHASE. A strictly negative value means that the element has reached temperature T2PHASE but not yet T1PHASE. ⁄ History variable Description 1-6 Back stress 7 Temperature at last time step 8 Yield indicator: 1 if yielding, else 0 9 Welding material indicator: 0 for ghost material, else 1 10 Maximum temperature reached 11 Average temperature rate going from T2PHASE to T1PHASE *MAT_271 This is material type 271. This model is used to analyze the compaction and sintering of cemented carbides and the model is based on the works of Brandt (1998). This material is only available for solid elements. Card 1 1 Variable MID 2 RO 3 4 5 6 7 8 P11 P22 P33 P12 P23 P13 Type A8 F F F F F F F Default none none none none none none none none Card 2 Variable 1 E0 2 LCK Type F F 3 PR F 4 5 6 LCX LCY LCC F F F 7 L F 8 R F Default none none none none none none none none Card 3 Variable 1 CA Type F 2 CD F 3 CV F 4 P F 5 6 7 8 LCH LCFI SINT TZRO F F F F Default none none none none none none 0.0 none Sintering Card 1. Additional card for SINT = 1. Card 4 1 2 3 4 5 6 7 8 Variable LCFK LCFS2 DV1 DV2 DS1 DS2 OMEGA RGAS Type F F F F F F F F Default none none none none none none none none Sintering Card 2. Additional card for SINT = 1. Card 5 1 2 3 4 5 6 Variable LCPR LCFS3 LCTAU ALPHA LCFS1 GAMMA Type F F F F F F 7 L0 F 8 LCFKS F Default none none none none none none none none VARIABLE DESCRIPTION MID RO PIJ E0 LCK PR LCX LCY Material identification. A unique number or label not exceeding 8 characters must be specified. Mass density. Initial compactness tensor Pij Initial anisotropy variable e (value between 1 and 2) Load curve for bulk modulus K as function of relative density d Poisson’s ratio Load curve for hydrostatic compressive yield X as function of relative density d Load curve for uniaxial compressive yield Y as function of relative density d LCC Load curve for shear yield C0 as function of relative density d L R CA CD CV P LCH LCFI Yield surface parameter L relating hydrostatic compressive yield to point on hydrostatic axis with maximum strength Yield surface parameter R governing the shape of the yield surface Hardening parameter ca Hardening parameter cd Hardening parameter cv Hardening exponent p Load curve giving back stress parameter H as function of hardening parameter e. Load curve giving plastic strain evolution angle ϕ as function of relative volumetric stress. SINT Activate sintering EQ.0.0: Sintering off EQ.1.0: Sintering on Absolute zero temperature T0 Load curve fK for viscous compliance as function of relative density d Load curve fS2 for viscous compliance as function of temperature T Volume diffusion coefficient dV1 Volume diffusion coefficient dV2 Surface diffusion coefficient dS1 Surface diffusion coefficient dS2 TZRO LCFK LCFS2 DV1 DV2 DS1 DS2 OMEGA Blending parameter ω RGAS LCPR Universal gas constant Rgas Load curve for viscous Poisson’s ratio ν as function of relative density d LCFS3 LCTAU ALPHA LCFS1 Load curve fS3 for evolution of mobility factor as function of temperature T Load curve for relaxation time τ as function of temperature T Thermal expansion coefficient α Load curve fS1 for sintering stress scaling as function of relative density d GAMMA Surface energy density γ affecting sintering stress L0 Grain size l0 affecting sintering stress LCFKS Load curve fKS scaling bulk modulus as function of temperature T Remarks: This model is intended to be used in two stages. During the first step the compaction of a powder specimen is simulated after which the results are dumped to file, and in a subsequent step the model is restarted for simulating sintering of the compacted specimen. In the following, an overview of the two different models is given, for a detailed description we refer to Brandt (1998). The progressive stiffening in the material during compaction makes it more or less necessary to run double precision and with constraint contacts to avoid instabilities, unfortunately this currently limitates the use of this material to the smp version of LS-DYNA. The powder compaction model makes use of a multiplicative split of the deformation gradient into a plastic and elastic part according to 𝐅 = 𝐅𝑒𝐅𝑝 where the plastic deformation gradient maps the initial reference configuration to an intermediate relaxed configuration 𝛿𝐱̃ = 𝐅𝑝𝛿𝐗 and subsequently the elastic part maps this onto the current loaded configuration 𝛿𝐱 = 𝐅𝑒𝛿𝐱̃ The compactness tensor is introduced that maps the intermediate configuration onto a virtual fully compacted configuration and we define the relative density as 𝛿𝐱̅ = 𝐏𝛿𝐱̃ 𝑑 = det𝐏 = 𝜌̅ where 𝜌 and 𝜌̅ denotes the current and fully compacted density, respectively. The elastic properties depend highly on the relative density through the bulk modulus 𝐾(𝑑) but the Poisson’s ratio is assumed constant. Y(d) nε φ(J1/X(d)) nε C0(d) Y(d) max=(L- -J1 = σVM -X(d)L -J1 - X(d) The yield surface is represented by two functions in the Rendulic plane according to 𝜎𝑌(𝑑) = ⎧𝐶0(𝑑) − 𝐶1(𝑑)𝐽1 − 𝐶2(𝑑)𝐽1 {{ √[(𝐿 − 1)𝑋(𝑑)]2 − [𝐽1 − 𝐿𝑋(𝑑)]2 ⎨ {{ ⎩ 𝐽1 ≥ 𝐿𝑋(𝑑) 𝐽1 < 𝐿𝑋(𝑑) and is in this way capped in both compression and tension, here 𝐽1 = 3𝜎 𝑚 = 𝑇𝑟(σ). The polynomial coefficients in the expression above are chosen to give continuity at 𝐽1 = 𝐿𝑋(𝑑) and to give the uniaxial compressive strength Y(d). Yielding is assumed to occur when the equivalent stress (note the definition) equals the yield stress where 𝜎eq = 𝜎𝑉𝑀 √3 = √ 𝐬: 𝐬 ≤ 𝜎𝑌(𝑑) 𝐬 = σ − 𝜎 𝑚𝐈 ⏟⏟⏟⏟⏟ σ𝑑 − κ in which the last term is the back stress to be dealt with below. The yield surface does not depend on the third stress invariant. The plastic flow is non-assosiated and its direction is given by where 𝐧𝜀 = ( cos𝜑 −sin𝜑 sin𝜑 cos𝜑 ) 𝐧 ∂𝜎𝑌 ⎟⎟⎞ ∂𝐽1 1 ⎠ 𝐧 = 𝜎𝑌(𝑑) ⎜⎜⎛ 𝜎max ⎝ is the normal to the yield surface as depicted in the Rendulic plane above (note the sign of J1). The angle φ is a function of and defined only for positive values of the relative volumetric stress J1/X(d)>0, for negative values φ is determined internally to achieve smoothness in the plastic flow direction and such that avoid numerical problems at the tensile cap point. The above equations are for illustrative purposes, from now on the plastic flow direction is generalized to a second order tensor. The plastic flow rule is then ε̇𝑝 = 𝜆̇𝐧𝜀, 𝑚 = 𝜀̇𝑝 𝑇𝑟(ε̇𝑝), 𝑑 = ε̇𝑝 − 𝜀̇𝑝 ε̇𝑝 𝑚𝐈 The evolution of the compactness tensor is directly related to the evolution of plastic strain as 𝐏̇ = − (ε̇𝑝𝐏 + 𝐏ε̇𝑝) and thus the relative density is given by 𝑑 ̇= −3𝜀̇𝑝 𝑚𝑑 . The back stress is assumed coaxial with the deviatoric part of the compactness tensor and given by κ = 𝐽1𝐻(𝑒) (𝐏 − 𝑇𝑟(𝐏) 𝐈) where e is a measure of intensity of anisotropy. This takes a value between 1 and 2 and evolves with plastic strain and plastic work according to 𝒆 ̇ = 𝑐𝑎√ where 𝑑: 𝛆̇𝑝 𝛆̇𝑝 𝑑 − 𝑐𝑣𝐽1𝜀̇𝑝 𝑚𝑊(𝑑, 𝐽1) + 𝑐𝑑𝛆̇𝑝 𝑑: 𝛔𝑊(𝑑, 𝐽1) 𝑊(𝑑, 𝐽1) = − [ 𝐽1 𝑋(𝑑) ] ∫ 𝑑0 𝑋(𝜉 ) 3𝜉 𝑑𝜉 and d0 is the density in the initial uncompressed configuration. The stress update is completed by the rate equation of stress where C(d) is the elastic constitutive matrix. 𝝈̇ = 𝐂(𝑑): (ε̇ − ε̇𝑝) The sintering model is a thermo and viscoelastic model where the evolution of the mean and deviatoric stress can be written as 𝜎̇ 𝑚 = 3𝐾𝑠(𝜀̇𝑚 − 𝜀̇𝑇 − 𝜀̇𝑝 𝑚) σ̇ 𝑑 = 2𝐺𝑠(ε̇𝑑 − ε̇𝑝 𝑑) The thermal strain rate is given by the thermal expansion coefficient as 𝜀̇𝑇 = 𝛼𝑇̇ and the bulk and shear modulus are the same as for the compaction model with the exception that they are scaled by a temperature curve 𝐾𝑠 = 𝑓𝐾𝑆(𝑇)𝐾(𝑑) 𝐺𝑠 = 3(1 − 2𝜈) 2(1 + 𝜈) 𝐾𝑠 The inelastic strain rates are different from the compaction model and is here given by ε̇𝑝 = 𝝈𝑑 2𝐺𝑣 + 𝜎 𝑚 − 𝜎 𝑠 3𝐾𝑣 𝐈 which results in a viscoelastic behavior depending on the viscous compliance and sintering stress. The viscous bulk compliance can be written 𝐾𝑣 = 3𝑓𝐾(𝑑) {𝑑𝑉1exp [− 𝑑𝑉2 𝑅𝑔𝑎𝑠(𝑇 − 𝑇0) ] + 𝜔𝑑𝑆1exp [− 𝑑𝑆2 𝑅𝑔𝑎𝑠(𝑇 − 𝑇0) ]} [1 + 𝑓𝑆2(𝑇)𝜉 ] from which the viscous shear compliance is modified with aid of the viscous Poisson’s ratio 𝐺𝑣 = 2[1 + 𝜈𝑣(𝑑)] 3[1 − 2𝜈𝑣(𝑑)] 𝐾𝑣 . The mobility factor ξ evolves with temperature according to and the sintering stress is given as 𝜉 ̇ = 𝑓𝑆3(𝑇)𝑇̇ − 𝜉 𝜏(𝑇) 𝜎 𝑠 = 𝑓𝑆1(𝑑) 𝑙0 . All this is accompanied with, again, the evolution of relative density given as 𝑑 ̇= −3𝜀̇𝑝 𝑚𝑑 *MAT_RHT This is material type 272. This model is used to analyze concrete structures subjected to impulsive loadings, see Riedel et.al. (1999) and Riedel (2004). Card 1 1 2 3 4 5 Varriable MID RO SHEAR ONEMPA EPSF Type A8 Card 2 Variable Type 1 A F Card 3 1 F 2 N F 2 Varriable E0C E0T Type F Card 4 1 F 2 Variable GC* GT* Type F F Card 5 1 Variable GAMMA Type F 2 A1 F F 3 FC F 3 EC F 3 XI F 3 A2 F 6 B0 F 6 Q0 F 6 7 B1 F 7 B F 7 F 4 F 5 FS* FT* F 5 BETAC BETAT PTF F 5 D2 F 5 F 6 EPM F 6 F 7 AF F 7 F 4 ET F 4 D1 F 4 A3 F 8 T1 F 8 T2 F 8 8 NF F 8 PEL PCO NP ALPHA0 F F F MID RO SHEAR ONEMPA *MAT_272 DESCRIPTION Material identification. A unique number or label not exceeding 8 characters must be specified. Mass density. Elastic shear modulus Unit conversion factor defining 1 Mpa in the pressure units used. It can also be used for automatic generation of material parameters for a given compressive strength. EQ.0: Defaults to 1.0 EQ.-1: Parameters generated in m, s and kg (Pa) EQ.-2: Parameters generated in mm, s and tonne (MPa) EQ.-3: Parameters generated in mm, ms and kg (GPa) EQ.-4: Parameters generated in in, s and dozens of slugs (psi) EQ.-5: Parameters generated in mm, ms and g (MPa) EQ.-6: Parameters generated in cm, μs and g (Mbar) EQ.-7: Parameters generated in mm, ms and mg (kPa) EPSF Eroding plastic strain (default is 2.0) B0 B1 T1 A N FC FS* FT* Q0 B T2 Parameter for polynomial EOS Parameter for polynomial EOS Parameter for polynomial EOS Failure surface parameter 𝐴 Failure surface parameter 𝑁 Compressive strength. Relative shear strength Relative tensile strength Lode angle dependence factor Lode angle dependence factor Parameter for polynomial EOS VARIABLE DESCRIPTION E0C E0T EC ET BETAC BETAT PTF GC* GT* XI D1 D2 EPM AF NF Reference compressive strain rate Reference tensile strain rate Break compressive strain rate Break tensile strain rate Compressive strain rate dependence exponent (optional) Tensile strain rate dependence exponent (optional) Pressure influence on plastic flow in tension (default is 0.001) Compressive yield surface parameter Tensile yield surface parameter Shear modulus reduction factor Damage parameter Damage parameter Minimum damaged residual strain Residual surface parameter Residual surface parameter GAMMA Gruneisen gamma A1 A2 A3 PEL PCO NP Hugoniot polynomial coefficient Hugoniot polynomial coefficient Hugoniot polynomial coefficient Crush pressure Compaction pressure Porosity exponent ALPHA Initial porosity *MAT_272 In the RHT model, the shear and pressure part is coupled in which the pressure is described by the Mie-Gruneisen form with a polynomial Hugoniot curve and a p-α compaction relation. For the compaction model, we define a history variable representing the porosity 𝛼 that is initialized to 𝛼0 > 1. This variable represents the current fraction of density between the matrix material and the porous concrete and will decrease with increasing pressure, i.e., the reference density is expressed as 𝛼𝜌. The evolution of this variable is given as 𝛼(𝑡) = max ⎜⎛1, min ⎝ ⎡1 + (𝛼0 − 1) ( ⎢ ⎣ where 𝑝(𝑡) indicates the pressure at time t. This expression also involves the initial pore crush pressure 𝑝el, compaction pressure 𝑝comp and porosity exponent 𝑁. For later use, we define the cap pressure, or current pore crush pressure, as 𝛼0, min𝑠≤𝑡 ⎟⎞ ⎠ ) 𝑝comp − 𝑝(𝑠) 𝑝comp − 𝑝el }⎫ ⎤ ⎥ ⎭}⎬ ⎦ {⎧ ⎩{⎨ 𝑝𝑐 = 𝑝comp − (𝑝comp − 𝑝el) ( 1/𝑁 ) 𝛼 − 1 𝛼0 − 1 The remainder of the pressure (EOS) model is given in terms of the porous density 𝜌 and specific internal energy 𝑒 (wrt the porous density). Depending on user inputs, it is either governed by (𝐵0 > 0) 𝑝(𝜌, 𝑒) = (𝐵0 + 𝐵1𝜂)𝛼𝜌𝑒 + 𝐴1𝜂 + 𝐴2𝜂2 + 𝐴3𝜂3 𝜂 > 0 { 𝐵0𝛼𝜌𝑒 + 𝑇1𝜂 + 𝑇2𝜂2 𝜂 < 0 or (𝐵0 = 0) together with 𝑝(𝜌, 𝑒) = Γ𝜌𝑒 + 𝑝𝐻(𝜂) = 𝐴1𝜂 + 𝐴2𝜂2 + 𝐴3𝜂3 𝑝𝐻(𝜂) [1 − Γ𝜂] 𝜂(𝜌) = 𝛼𝜌 𝛼0𝜌0 − 1 . For the shear strength description we use 𝑝∗ = 𝑓𝑐 . as the pressure normalized with the compressive strength parameter. We also use 𝐬 to denote the deviatoric stress tensor and 𝜀̇𝑝 the plastic strain rate. The effective plastic strain is thus denoted ε𝑝 and can be viewed as such in the post processor of choice. For a given stress state and rate of loading, the elastic-plastic yield surface for the RHT model is given by 𝜎𝑦(𝑝∗, 𝐬, 𝜀̇𝑝, 𝜀𝑝 ∗) = 𝑓𝑐𝜎𝑦 ∗(𝑝∗, 𝐹𝑟(𝜀̇𝑝, 𝑝∗), 𝜀𝑝 ∗)𝑅3(𝜃, 𝑝∗) and is the composition of two functions and the compressive strength parameter 𝑓𝑐. The first describes the pressure dependence for principal stress conditions 𝜎1 < 𝜎2 = 𝜎3 and is expressed in terms of a failure surface and normalized plastic strain as 𝜎𝑦 ∗(𝑝∗, 𝐹𝑟, 𝜀𝑝 ∗) = 𝜎𝑓 ∗ ( 𝑝∗ , 𝐹𝑟) 𝛾 with The failure surface is given as 𝛾 = 𝜀𝑝 ∗ + (1 − 𝜀𝑝 ∗)𝐹𝑒𝐹𝑐 . ∗(𝑝∗, 𝐹𝑟) = 𝜎𝑓 ⎡𝑝∗ − ⎢ ⎣ 𝐹𝑟 + ( 𝐹𝑟 −1 𝑛⁄ ) ⎤ ⎥ ⎦ + 3𝑝∗ (1 − ∗ 𝑓𝑠 𝑄1 ) − 3𝑝∗ ( 𝑄2 − ∗ 𝑓𝑠 𝑄1𝑓𝑡 ∗) ∗ 𝐹𝑟𝑓𝑠 𝑄1 ∗ 𝐹𝑟𝑓𝑠 𝑄1 ⎧ { { { { { { { { { { { ⎨ { { { { { { { { { { { ⎩ 3𝑝∗ ≥ 𝐹𝑟 𝐹𝑟 > 3𝑝∗ ≥ 0 ∗ 0 > 3𝑝∗ > 3𝑝𝑡 3𝑝𝑡 ∗ > 3𝑝∗ ∗ = in which 𝑝𝑡 factor and 𝐹𝑟𝑄2𝑓𝑠 ∗ ∗𝑓𝑡 ∗−𝑄2𝑓𝑠 ∗) 3(𝑄1𝑓𝑡 is the failure cut-off pressure, 𝐹𝑟 is a dynamic increment 𝑄1 = 𝑅3 ( , 0) 𝑄2 = 𝑄(𝑝∗) ∗ are the tensile and shear strength of the concrete relative In these expressions, 𝑓𝑡 to the compressive strength 𝑓𝑐 and the Q values are introduced to account for the tensile and shear meridian dependence. Further details are given in the following. ∗ and 𝑓𝑠 To describe reduced strength on shear and tensile meridian the factor 𝑅3(𝜃, 𝑝∗) = 2(1 − 𝑄2)cos𝜃 + (2𝑄 − 1)√4(1 − 𝑄2)cos2𝜃 + 5𝑄2 − 4𝑄 4(1 − 𝑄2)cos2𝜃 + (1 − 2𝑄)2 is introduced, where 𝜃 is the Lode angle given by the deviatoric stress tensor s as cos3𝜃 = 27 det(𝐬) 2𝜎̅̅̅̅̅(𝐬)3 𝜎̅̅̅̅̅(𝐬) = √ 𝐬: 𝐬 . The maximum reduction in strength is given as a function of relative pressure Finally, the strain rate dependence is given by 𝑄 = 𝑄(𝑝∗) = 𝑄0 + 𝐵𝑝∗ . 𝐹𝑟(𝜀̇𝑝, 𝑝∗) = in which 𝑐 − 𝐹𝑟 ⎧ { { ⎨ { { ⎩ 𝐹𝑟 3𝑝∗ − 𝐹𝑟 ∗ (𝐹𝑟 𝑐 + 𝐹𝑟 𝑡𝑓𝑡 𝐹𝑟 𝐹𝑟 𝑡 − 𝐹𝑟 𝑐) 𝐹𝑟 ∗ 𝑐 > 3𝑝∗ ≥ −𝐹𝑟 𝑡𝑓𝑡 3𝑝∗ ≥ 𝐹𝑟 𝑡𝑓𝑡 −𝐹𝑟 ∗ > 3𝑝∗ 𝑡(𝜀̇𝑝) = 𝐹𝑟 ⎧ {{{ ⎨ {{{ ⎩ ⎜⎜⎛ 𝜀̇𝑝 𝑡⁄ 𝜀̇0 ⎝ 𝛾𝑐 𝛽𝑐 𝑡⁄ ⎟⎟⎞ ⎠ √𝜀̇𝑝 𝑡⁄ 𝜀̇𝑝 ≥ 𝜀̇𝑝 𝑡⁄ 𝜀̇𝑝 > 𝜀̇𝑝 . The parameters involved in these expressions are given as (𝑓𝑐 is in MPa below) 𝛽𝑐 = 𝛽𝑡 = 20 + 3𝑓𝑐 20 + 𝑓𝑐 and 𝛾𝑐/𝑡 is determined from continuity requirements, but it is also possible to choose the rate parameters via inputs. The elastic strength parameter used above is given by 𝐹𝑒(𝑝∗) = ⎧ { { { ⎨ { { { ⎩ ∗ − 𝑔𝑐 ∗ 𝑔𝑐 3𝑝∗ − 𝐹𝑟 ∗ 𝑐𝑔𝑐 ∗𝑓𝑡 ∗ + 𝐹𝑟 𝑡𝑔𝑡 𝑐𝑔𝑐 𝐹𝑟 ∗ 𝑔𝑡 3𝑝∗ ≥ 𝐹𝑟 ∗ 𝑐𝑔𝑐 ∗ (𝑔𝑡 ∗ − 𝑔𝑐 ∗) 𝐹𝑟 𝑐𝑔𝑐 ∗ > 3𝑝∗ ≥ −𝐹𝑟 𝑡𝑔𝑡 ∗ ∗𝑓𝑡 −𝐹𝑟 𝑡𝑔𝑡 ∗𝑓𝑡 ∗ > 3𝑝∗ while the cap of the yield surface is represented by 𝐹𝑐(𝑝∗) = 𝑝∗ ≥ 𝑝𝑐 ∗ √1 − ( ∗ 𝑝∗ − 𝑝𝑢 ∗ ) ∗ − 𝑝𝑢 𝑝𝑐 ∗ > 𝑝∗ ≥ 𝑝𝑢 ∗ 𝑝𝑐 ∗ > 𝑝∗ 𝑝𝑢 ⎧ {{{ ⎨ {{{ ⎩ where 𝑝𝑐 𝑓𝑐 + ∗ = 𝑝𝑐 ∗ 𝑐𝑔𝑐 𝐹𝑟 𝐺∗𝜀𝑝 𝑓𝑐 ∗ = 𝑝𝑢 The hardening behavior is described linearly with respect to the plastic strain, where , 1 ∗ = min 𝜀𝑝 𝜀𝑝 ⎟⎞ ⎜⎛ 𝜀𝑝 ⎠ ⎝ ∗)(1 − 𝐹𝑒𝐹𝑐) 𝜎𝑦(𝑝∗, 𝐬, 𝜀̇𝑝, 𝜀𝑝 𝛾3𝐺∗ ℎ = 𝜀𝑝 here 𝐺∗ = 𝜉𝐺 where 𝐺 is the shear modulus of the virgin material and 𝜉 is a reduction factor representing the hardening in the model. When hardening states reach the ultimate strength of the concrete on the failure surface, damage is accumulated during further inelastic loading controlled by plastic strain. To this end, the plastic strain at failure is given as 𝑓 = 𝜀𝑝 ⎧ {{{{ {{{{ ⎨ ⎩ 𝐷1[𝑝∗ − (1 − 𝐷)𝑝𝑡 ∗]𝐷2 𝑝∗ ≥ (1 − 𝐷)𝑝𝑡 ∗ + ( 𝜀𝑝 (1 − 𝐷)𝑝𝑡 ∗ + ( 𝜀𝑝 𝐷1 ) ⁄ 𝐷2 ) 𝜀𝑝 𝐷1 ⁄ 𝐷2 > 𝑝∗ The damage parameter is accumulated with plastic strain according to 𝜀𝑝 𝐷 = ∫ 𝜀𝑝 𝑑𝜀𝑝 𝜀𝑝 and the resulting damage surface is given as 𝜎𝑑(𝑝∗, 𝐬, 𝜀̇𝑝) = ⎧ {{{ ⎨ {{{ ⎩ 𝜎𝑦(𝑝∗, 𝐬, 𝜀̇𝑝, 1)(1 − 𝐷) + 𝐷𝑓𝑐𝜎𝑟 ∗(𝑝∗) 0 ≤ 𝑝∗ 𝜎𝑦(𝑝∗, 𝐬, 𝜀̇𝑝, 1) (1 − 𝐷 − 𝑝∗ ∗) 𝑝𝑡 (1 − 𝐷)𝑝𝑡 ∗ ≤ 𝑝∗ < 0 where ∗(𝑝∗) = 𝐴𝑓 {𝑝∗}𝑛𝑓 𝜎𝑟 Plastic flow occurs in the direction of deviatoric stress, i.e., ε̇𝑝~𝐬 but for tension there is an option to set the parameter PFC to a number corresponding to the influence of plastic volumetric strain. If 𝜆 ≤ 1 is used to denote this parameter, then for the special case of 𝜆 = 1 ε̇𝑝~𝐬 − 𝑝𝐈 This was introduced to reduce noise in tension that was observed on some test problems. A failure strain can be used to erode elements with severe deformation which by default is set to 200%. For simplicity, automatic generation of material parameters is available via ONEMPA.LT.0, then no other parameters are needed. If FC.EQ.0 then the 35 MPa strength concrete in Riedel (2004) is generated in the units specified by the value of ONEMPA. For FC.GT.0 then FC specifies the actual strength of the concrete in the units specified by the value of ONEMPA. The other parameters are generated by interpolating between the 35 MPa and 140 MPa strength concretes as presented in Riedel (2004). Any automatically generated parameter may be overridden by the user if motivated, one of these parameters may be the initial porosity ALPHA0 of the concrete. For post-processing, the following history variables may be of interest History variable #2 Internal energy per volume (ρe) History variable #3 Porosity value (α) History variable #4 Damage value (D) or as an alternative use a material history list *DEFINE_MATERIAL_HISTORIES Properties Label Attributes Description Damage - - - - Damage value 𝐷 *MAT_CONCRETE_DAMAGE_PLASTIC_MODEL *MAT_CDPM This is material type 273. CDPM is a damage plastic concrete model based on work published in Grassl et al. (2011, 2013) and Grassl and Jirásek (2006). This model is aimed to simulations where failure of concrete structures subjected to dynamic loadings is sought. It describes the characterization of the failure process subjected to multi-axial and rate-dependent loading. The model is based on effective stress plasticity and with a damage model based on both plastic and elastic strain measures. This material model is available only for solids. There are a lot of parameters for the advanced user but note that most of them have default values that are based on experimental tests. They might not be useful for all types of concrete and all types of load paths but they are values that can be used as a good starting point. If the default values are not good enough the theory chapter at the end of the parameter description can be of use. History variables of interest are: 1 – kappa, 𝜅, see equations below 15 – damage in tension, 𝜔𝑡, see equations below 16 – damage in compression, 𝜔𝑐, see equations below More details on this material can be found on: http://petergrassl.com/Research/DamagePlasticity/CDPMLSDYNA/index.html Card 1 1 Variable MID 2 RO Type A8 F 3 E F 4 PR F 5 6 ECC QH0 F F 7 FT F 8 FC F Default none none none 0.2 AUTO 0.3 none none Card 2 Variable 1 HP Type F 2 AH F 3 BH F 4 CH F 5 DH F 6 AS F 7 DF F 8 FC0 F Default 0.5 0.08 0.003 2.0 1.0E-6 15.0 0.85 AUTO Card 3 1 Variable TYPE Type F 2 BS F 3 WF 4 5 6 7 8 WF1 FT1 STRFLG FAILFLG EFC F F F F F F Default 0.0 1.0 none 0.15*WF 0.3*FT 0.0 0.0 1.0E-4 VARIABLE DESCRIPTION MID RO E PR ECC Material identification. A unique number or label not exceeding 8 characters must be specified. Mass density. Young’s modulus. The sign determines if an anisotropic (E positive, referred to as ISOFLAG = 0 in the remarks) or an isotropic (E negative, referred to as ISOFLAG = 1 in the remarks) damage formulation is used. The Young’s modulus is taken as the absolute value of this parameter. Poissons ratio Eccentricity parameter. EQ.0.0: ECC is calculated from Jirásek and Bazant (2002) as ECC = 1 + 𝜖 2 − 𝜖 , 𝜖 = 𝑓𝑡(𝑓𝑏𝑐 𝑓𝑏𝑐(𝑓𝑐 2 − 𝑓𝑐 2 − 𝑓𝑡 2) 2) , 𝑓𝑏𝑐 = 1.16𝑓𝑐 QH0 Initial hardening defined as FC0/FC where FC0 is the compressive stress at which the initial yield surface is reached. Default = 0.3 FT FC HP AH BH CH DH AS DF FC0 Uniaxial tensile strength (stress) Uniaxial compression strength (stress) Hardening parameter. Default is HP = 0.5 which is the value used in Grassl et al. (2011) for strain rate dependent material response (STRFLG = 1). For applications without strain rate effect (STRFLG = 0) a value of HP = 0.01 is recommended, which has been used in Grassl et al. (2013). Hardening ductility parameter 1 Hardening ductility parameter 2 Hardening ductility parameter 3 Hardening ductility parameter 4 Ductility parameter during damage Flow rule parameter Rate dependent parameter. if STRFLG = 1. Recommended value is 10 MPa, which has to be entered consistently with the system of units used. Only needed TYPE Flag for damage type. EQ.0.0: Linear damage formulation EQ.1.0: Bi-linear damage formulation EQ.2.0: Exponential damage formulation EQ.3.0: No damage The best results are obtained with the bi-linear formulation. Damage ductility exponent during damage. Default = 1.0 threshold value formulation. Tensile Parameter controlling tensile softening branch for exponential tensile damage formulation. linear damage for Tensile threshold value for the second part of the bi-linear damage formulation. Default = 0.15 × WF BS WF WF1 FT1 strength Tensile formulation. Default = 0.3 × FT STRFLG Strain rate flag. threshold value for bi-linear damage EQ.1.0: Strain rate dependent EQ.0.0: No strain rate dependency. FAILFLG Failure flag. EQ.0.0: Not active ⇒ No erosion. GT.0.0: Active and element will erode if wt and wc is equal to 1 in FAIFLG percent of the integration points. If FAIL- FLG = 0.60, 60% of all integration points must fail be- fore erosion. EFC Parameter controlling compressive damage softening branch in the exponential compressive damage formulation. Default = 1.0E-4 Remarks: The stress for the anisotropic damage plasticity model (E positive, ISOFLAG = 0) is defined as 𝝈 = (1 − 𝜔𝑡)𝝈𝑡 + (1 − 𝜔𝑐)𝝈𝑐 where 𝝈𝑡 and 𝝈𝑐 are the positive and negative part of the effective stress 𝝈eff determined in the principal stress space. The scalar functions 𝜔𝑡 and 𝜔𝑐 are damage parameters. The stress for the isotropic damage plasticity model (E negative, ISOFLAG = 1) is defined as 𝝈 = (1 − 𝜔𝑡)𝝈eff The effective stress 𝝈𝐞𝐟𝐟 is defined according to the damage mechanics convention as 𝝈𝐞𝐟𝐟 = 𝑫𝒆: (𝜺 − 𝜺𝒑) Plasticity: The yield surface is described by the Haigh-Westergaard coordinates: the volumetric effective stress 𝜎𝑣, the norm of the deviatoric effective stress 𝜌 and the Lode angle 𝜃, and it is given by 𝑓𝑝(𝜎𝑣, 𝜌, 𝜃, 𝜅) = [1 − 𝑞1(𝜅)] ⎡ ⎢⎢⎢ ⎣ − 𝑞1 2(𝜅)𝑞2 2(𝜅) . ⎜⎜⎛ 𝜌 √6𝑓𝑐 ⎝ + 𝜎𝑣 ⎟⎟⎞ 𝑓𝑐 ⎠ + √ 𝑓𝑐 ⎤ ⎥⎥⎥ ⎦ + 𝑚0𝑞1(𝜅)2𝑞2(𝜅) ⎡ 𝜌 ⎢ √6𝑓𝑐 ⎣ 𝑟(cos 𝜃) + 𝜎𝑣 ⎤ ⎥ 𝑓𝑐 ⎦ The variables 𝑞1 and 𝑞2 are dependent on the hardening variable 𝜅. The parameter 𝑓𝑐 is the uniaxial compressive strength. The shape of the deviatoric section is controlled by the function 𝑟(cos 𝜃) = 4(1 − 𝑒2) cos2 𝜃 + (2𝑒 − 1)2 2(1 − 𝑒2) cos 𝜃 + (2𝑒 − 1)√4(1 − 𝑒2) cos2 𝜃 + 5𝑒2 − 4𝑒 where 𝑒 is the eccentricity parameter (ECC). The parameter 𝑚0 is the friction parameter and it is defined as 𝑚0 = where 𝑓𝑡 is the tensile strength. 3(𝑓𝑐 2 − 𝑓𝑡 𝑓𝑐𝑓𝑡 ) 𝑒 + 1 The flow rule is non-associative which means that the direction of the plastic flow is not normal to the yield surface. This is important for concrete since an associative flow rule would give an overestimated maximum stress. The plastic potential is given by 𝑔(𝜎𝑣, 𝜌, 𝜅) = {⎧ ⎩{⎨ [1 − 𝑞1(𝜅)] ⎜⎛ 𝜌 √6𝑓𝑐 ⎝ + 𝜎𝑣 ⎟⎞ 𝑓𝑐 ⎠ + √ }⎫ 𝑓𝑐⎭}⎬ + 𝑞1(𝜅) ⎜⎛𝑚0𝜌 √6𝑓𝑐 ⎝ + 𝑚𝑔(𝜎𝑣, 𝜅) 𝑓𝑐 ⎟⎞ ⎠ where and 𝑚𝑔(𝜎𝑣, 𝜅) = 𝐴𝑔(𝜅)𝐵𝑔(𝜅)𝑓𝑐𝑒 𝜎𝑣−𝑞2𝑓𝑡/3 𝐵𝑔𝑓𝑐 𝐴𝑔 = 3𝑓𝑡𝑞2(𝜅) 𝑓𝑐 + 𝑚0 , 𝐵𝑔 = 𝑞2(𝜅) 1 + 𝑓𝑡/𝑓𝑐 ln 𝐴𝑔 3𝑞2 + 𝑚0 + ln ( 𝐷𝑓 + 1 2𝐷𝑓 − 1 ) The hardening laws 𝑞1 and 𝑞2 control the shape of the yield surface and the plastic potential, and they are defined as 𝑞1(𝜅) = 𝑞ℎ0 + (1 − 𝑞ℎ0)(𝜅3 − 3𝜅2 + 3𝜅) − 𝐻𝑝(𝜅3 − 3𝜅2 + 2𝜅), 𝜅 < 1 𝑞1(𝜅) = 1, 𝜅 ≥ 1 𝑞2(𝜅) = 1, 𝜅 < 1 𝑞2(𝜅) = 1 + 𝐻𝑝(𝜅 − 1), 𝜅 ≥ 1 The evolution for the hardening variable is given by 4𝜆̇ cos2 𝜃 𝑥ℎ(𝜎𝑣) It sets the rate of the hardening variable to the norm of the plastic strain rate scaled by a ductility measure which is defined below as 𝑑𝑔 𝑑𝜎 𝜅̇ = ∥ ∥ − 𝑥ℎ(𝜎𝑣) = 𝐴ℎ − (𝐴ℎ − 𝐵ℎ)𝑒 𝑅ℎ 𝐹ℎ + 𝐷ℎ, 𝑅ℎ < 0 𝑅ℎ 𝐶ℎ, 𝑅ℎ ≥ 0 𝑥ℎ(𝜎𝑣) = 𝐸ℎ𝑒 And finally Damage: 𝐸ℎ = 𝐵ℎ − 𝐷ℎ, 𝐹ℎ = (𝐵ℎ − 𝐷ℎ)𝐶ℎ 𝐴ℎ − 𝐵ℎ Damage is initialized when the equivalent strain 𝜀̃ reaches the threshold value 𝜀0 = 𝑓𝑡 𝐸⁄ where the equivalent strain is defined as 𝜀̃ = 𝜀0𝑚0 ⎡ 𝜌 ⎢ 2 ⎣ √6𝑓𝑐 𝑟(𝑐𝑜𝑠𝜃) + 𝜎𝑉 ⎤ + ⎥ 𝑓𝑐 ⎦ 2𝑚0 𝜀0 4 ⎝ ⎜⎛ 𝜌 √6𝑓𝑐 𝑟(𝑐𝑜𝑠𝜃) + 𝜎𝑉 ⎟⎞ 𝑓𝑐 ⎠ + 2𝜌2 3𝜀0 2 2𝑓𝑐 √ √√ ⎷ Tensile damage is described by a stress-inelastic displacement law. For linear and exponential damage type the stress value 𝑓𝑡 and the displacement value 𝑤𝑓 must be defined. For the bi-linear type two additional parameters 𝑓𝑡1 and 𝑤𝑓1 must be defined, see figure below how the stress softening is controlled by the input parameters. 𝜎𝑡 𝑓𝑡 𝜎𝑡 𝑓𝑡 𝑓𝑡1 𝜎𝑡 𝑓𝑡 𝑤𝑓 𝜀𝑡ℎ 𝑤𝑓1 𝑤𝑓 𝜀𝑡ℎ 𝑤𝑓 𝜀𝑡ℎ The variable ℎ is a mesh-dependent measure used to convert strains to displacements. The variable 𝜀𝑡 is called the inelastic tensile strain and is defined as the sum of the irreversible plastic strain 𝜀𝑝 and the reversible strain 𝑤𝑡(𝜀 − 𝜀𝑝) (in compression 𝑤𝑐(𝜀 − 𝜀𝑝)). To get the influence of multi-axial stress states on the softening a damage ductility measure 𝑥𝑠 is added: Where 𝐴𝑠 and 𝐵𝑠 are input parameters, and 𝑥𝑠 = 1 + (𝐴𝑠 − 1)𝑅𝑠 𝐵𝑠 𝑅𝑠 = − √6𝜎𝑣 , 𝜎𝑣 < 0 𝑎𝑛𝑑 𝑅𝑠 = 0, 𝜎𝑣 > 0 The inelastic strain is then modified according: 𝜀𝑖 𝑥𝑠 𝜀𝑖 = Compressive damage is controlled by an exponential stress-inelastic strain law. Stress value 𝒇𝒄 and inelastic strain 𝜺𝒇𝒄 need to be specified, see figure below how the stress softening is controlled by the input parameters. A small value of 𝜺𝒇𝒄, i.e. 1.0E-4 (default), provides for a rather brittle form of damage. 𝜎𝑐 𝑓𝑐 𝐴𝑠 𝜀𝑓𝑐 𝜀𝑐 Strain rate: Concrete is strongly rate dependent. If the loading rate is increased, the tensile and compressive strength increase and are more prominent in tension then in compression. The dependency is taken into account by an additional variable 𝛼𝑟 ≥ 1. The rate dependency is included by scaling both the equivalent strain rate and the inelastic strain. The rate parameter is defined by 𝛼𝑟 = (1 − 𝑋compression) 𝛼𝑟𝑡 + 𝑋compression𝛼𝑟𝑐 Where 𝑋compression is continuous compression measure (= 1 means only compression, = 0 means only tension) and for tension we have 𝛼𝑟𝑡 = 𝛿𝑡 ⎧ ) ( {{{{{ {{{{{ 𝛽𝑡 ( ⎩ 𝜀̇max 𝜀̇𝑡0 𝜀̇max 𝜀̇𝑡0 ⎨ 𝜀̇max < 30 × 10−6𝑠−1 30 × 10−6 < 𝜀̇max < 1 𝑠−1 ) 𝜀̇max > 1 𝑠−1 where 𝛿𝑡 = 1 rate factor is given by 1+8𝑓𝑐/𝑓𝑐0 , 𝛽𝑡 = 𝑒6𝛿𝑡−2 and 𝜀̇𝑡0 = 1 × 10−6𝑠−1. For compression the corresponding 𝛼𝑟𝑐 = ⎧1 [𝑆 {{{{{ {{{{{ 𝛽𝑐 [ ⎩ ⎨ ] |𝜀̇min| 𝜀̇𝑐0 |𝜀̇min| 𝜀̇𝑐0 1.026𝛿𝑐 |𝜀̇min| < 30 × 10−6𝑠−1 30 × 10−6 < |𝜀̇min| < 1𝑠−1 ] | 𝜀̇min| > 30𝑠−1 where 𝛿𝑐 = 1 parameter. A recommended value is 10MPa. 5+9𝑓𝑐/𝑓𝑐0 , 𝛽𝑐 = 𝑒6.156𝛿𝑐−2 and 𝜀̇𝑐0 = 30 × 10−6𝑠−1. The parameter 𝑓𝑐0 is an input *MAT_PAPER This is material type 274. This is an orthotropic elastoplastic model for paper materials, based on Xia (2002) and Nygards (2009), and is available for solid and shell elements. Solid elements use a hyperelastic-plastic formulation, while shell elements use a hypoelastic-plastic formulation. Card 1 1 Variable MID 2 RO Type A8 F 3 E1 F 4 E2 F 5 E3 F 6 7 8 PR21 PR32 PR31 F F F Default none none none none none none none none Card 2 1 2 3 4 Variable G12 G23 G13 E3C Type F F F F 5 CC F TWOK F 6 7 8 Default none none none none none none ROT F 0.0 In plane Yield Surface Card 1. Card 3 1 2 3 4 5 6 7 8 Variable S01 A01 B01 C01 S02 A02 B02 C02 Type F F F F F F F F Default none none none none none none none none *MAT_274 Card 4 1 2 3 4 5 6 7 8 Variable S03 A03 B03 C03 S04 A04 B04 C04 Type F F F F F F F F Default none none none none none none none none In plane Yield Surface Card 3. Card 5 1 2 3 4 5 6 7 8 Variable S05 A05 B05 C05 PRP1 PRP2 PRP4 PRP5 Type F F F F F F F F Default none none none none 1/2 2/15 1/2 2/15 Out of Plane and Transverse Shear Yield Surface Card. Card 6 1 2 3 4 5 6 7 8 Variable ASIG BSIG CSIG TAU0 ATAU BTAU Type F F F F F F Default none none none none none none Card 7 1 2 Variable AOPT MACF Type F F *MAT_PAPER 3 XP F 4 YP F 5 ZP F 6 A1 F 7 A2 F 8 A3 F Default none none none none none none none none Orthotropic Parameter Card 2. Card 8 Variable 1 V1 Type F 2 V2 F 3 V3 F 4 D1 F 5 D2 F 6 D3 F 7 8 BETA F Default none none none none none none none VARIABLE DESCRIPTION MID RO Ei PRij Gij E3C CC Material identification. A unique number or label not exceeding 8 characters must be specified. Material density Young’s modulus in direction 𝐸𝑖. Elastic Poisson’s ratio 𝜈𝑖𝑗. Elastic shear modulus in direction 𝐺𝑖𝑗. Elastic compression parameter. Elastic compression exponent. TWOK Exponent in in-plane yield surface. ROT Option for 2D-solids (shell element form 13,14,15): EQ.0.0: No rotation of material axes (default). Direction of material axes are solely defined by AOPT and it is only possible to rotate in shell-plane. EQ.1.0: Rotate coordinate system around material 1-axis such that 2-axis coincides with shell normal. This rotation is done in addition to AOPT. EQ.2.0: Rotate coordinate system around material 2-axis such that 1-axis coincides with shell normal. This rotation is done in addition to AOPT. 𝑖th in-plane plasticity yield parameter. If S0i < 0 the absolute value of S0i is a curve number, see remarks. 𝑖th in-plane plasticity hardening parameter. 𝑖th in-plane plasticity hardening parameter. 𝑖th in-plane plasticity hardening parameter. Tensile plastic Poisson’s ratio in direction 1. Tensile plastic Poisson’s ratio in direction 2. Compressive plastic Poisson’s ratio in direction 1. Compressive plastic Poisson’s ratio in direction 2. Out-of-plane plasticity yield parameter. Out-of-plane plasticity hardening parameter. Out-of-plane plasticity hardening parameter. Transverse shear plasticity yield parameter. Transverse shear plasticity hardening parameter. Transverse shear plasticity hardening parameter. S0i A0i B0i C0i PRP1 PRP2 PRP4 PRP5 ASIG BSIG CSIG TAU0 ATAU BTAU AOPT Material axes option : EQ.0.0: locally orthotropic with material axes determined by element nodes 1, 2, and 4, as with *DEFINE_COORDI- NATE_NODES. EQ.1.0: locally orthotropic with material axes determined by a point in space and the global location of the element center; this is the a-direction. This option is for solid elements only. EQ.2.0: globally orthotropic with material axes determined by vectors defined below, as with *DEFINE_COORDI- NATE_VECTOR. EQ.3.0: locally orthotropic material axes determined by rotating the material axes about the element normal by an angle, BETA, from a line in the plane of the element defined by the cross product of the vector v with the element normal. EQ.4.0: locally orthotropic in cylindrical coordinate system with the material axes determined by a vector v, and an originating point, p, which define the centerline ax- is. This option is for solid elements only. LT.0.0: the absolute value of AOPT is a coordinate system ID number (CID on *DEFINE_COORDINATE_NODES, *DEFINE_COORDINATE_SYSTEM or *DEFINE_CO- ORDINATE_VECTOR). Available in R3 version of 971 and later. MACF Material axes change flag for brick elements: EQ.1: No change, default, EQ.2: switch material axes a and b, EQ.3: switch material axes a and c, EQ.4: switch material axes b and c. XP, YP, ZP Define coordinates of point 𝐩 for AOPT = 1 and 4. A1, A2, A3 Define components of vector 𝐚 for AOPT = 2. V1, V2, V3 Define components of vector 𝐯 for AOPT = 3 and 4. D1, D2, D3 Define components of vector 𝐝 for AOPT = 2. the element card, see *ELEMENT_SHELL_BETA or *ELEMENT_- SOLID_ORTHO. *MAT_PAPER BETA Remarks: The stress-strain relationship for solid elements is based on a multiplicative split of the deformation gradient into an elastic and a plastic part The elastic Green strain is formed as 𝐅 = 𝐅𝑒𝐅𝑝. 𝐄𝑒 = (𝐅𝑒 T𝐅𝑒 − 𝐈), and the 2nd Piola-Kirchhoff stress as 𝐒 = 𝐂𝐄𝑒, where the constitutive matrix is taken as orthotropic and can be represented in Voigt notation by its inverse as 𝐂−1 = 𝐸1 𝜐12 𝐸1 𝜐13 𝐸1 − − 𝜐21 𝐸2 𝐸2 𝜐23 𝐸2 − − 𝜐31 𝐸3 𝜐32 𝐸3 𝐸3 ⎤ ⎥ ⎥ ⎥ ⎥ ⎥ ⎥ ⎥ ⎥ . ⎥ ⎥ ⎥ ⎥ ⎥ ⎥ ⎥ ⎥ 𝐺13⎦ 𝐺12 𝐺23 − − ⎡ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎣ In out-of-plane compression the stress is modified according to 𝑆33 = 𝐶31𝐸11 𝑒 + 𝐶32𝐸22 𝑒 + { 𝑐 [1 − exp(−𝐶𝑐𝐸33 𝐸3 𝑒 , 𝐸3𝐸33 𝑒 )], 𝑒 ≥ 0, 𝑒 < 0. 𝐸33 𝐸33 Three yield surfaces are present: in-plane, out-of-plane, and transverse shear. The in- plane yield surface is given as 𝑓 = ∑ 𝑖=1 ⎡max(0, 𝑆: 𝑁𝑖) ⎢ 𝑓 ) 𝑞𝑖(𝜀𝑝 ⎣ 2𝑘 ⎤ ⎥ ⎦ − 1 ≤ 0 , with the 6 yield plane normals (in strain Voigt notation) 𝜐1𝑝 − √1 + 𝜐1𝑝 √1 + 𝜐1𝑝 𝑁1 = ⎡ ⎢ ⎣ 𝑁2 = ⎡− ⎢ ⎣ 𝜐2𝑝 √1 + 𝜐2𝑝 √1 + 𝜐2𝑝 ⎤ ⎥ ⎦ ⎤ ⎥ ⎦ , , 𝑁3 = [0 0 √2 𝑁4 = − ⎡ ⎢ √1 + 𝜐4𝑝 ⎣ − 0] , 𝜐4𝑝 √1 + 𝜐4𝑝 𝑁5 = − ⎡− ⎢ ⎣ 𝜐5𝑝 √1 + 𝜐5𝑝 √1 + 𝜐5𝑝 𝑁6 = −𝑁3. The yield planes describe the following states ⎤ ⎥ ⎦ ⎤ ⎥ ⎦ , , Each hardening function 𝑞𝑖 (note that 𝑞6 = 𝑞3) is given by a load curve if 𝑆𝑖 otherwise 0 < 0, 𝑞𝑖(𝜀𝑝 𝑓 ) = 𝑆𝑖 0 + 𝐴𝑖 0 tanh(𝐵𝑖 0𝜀𝑝 𝑓 ) + 𝐶𝑖 𝑓 . 0𝜀𝑝 The out-of-plane surface is given as 𝑔 = −𝑆33 𝑔) 𝐴𝜎 + 𝐵𝜎 exp(−𝐶𝜎𝜀𝑝 − 1 ≤ 0, and the transverse shear surface is ℎ = √𝑆13 2 + 𝑆23 𝜏0 + [𝐴𝜏 − min(0, 𝑆33) 𝐵𝜏]𝜀𝑝 − 1 ≤ 0. The flow rule is given by the evolution of the plastic deformation gradient where the plastic velocity gradient is given as 𝐅̇𝑝 = 𝐋𝑝𝐅𝑝, 𝐋𝑝 = 𝑓 𝜕𝑓 𝜕𝑆11 ⎡𝜀̇𝑝 ⎢ ⎢ 𝑓 𝜕𝑓 ⎢ 𝜀̇𝑝 ⎢ 𝜕𝑆12 ⎢ ⎢ ℎ 𝜕ℎ ⎢ 𝜀̇𝑝 𝜕𝑆13 ⎣ 𝑓 𝜕𝑓 𝜀̇𝑝 𝜕𝑆12 𝑓 𝜕𝑓 𝜀̇𝑝 𝜕𝑆22 ℎ 𝜕ℎ 𝜀̇𝑝 𝜕𝑆23 ℎ 𝜕ℎ 𝜀̇𝑝 𝜕𝑆13 ℎ 𝜕ℎ 𝜀̇𝑝 𝜕𝑆23 𝑔 𝜕𝑔 𝜀̇𝑝 ⎤ ⎥ ⎥ ⎥ , ⎥ ⎥ ⎥ ⎥ 𝜕𝑆33⎦ and where it is implicitly assumed that the involved derivatives in the expression of the velocity gradient is appropriately normalized. The stress-strain relationship for shell elements is based on an additive split of the rate of deformation into an elastic and a plastic part 𝐃 = 𝐃𝑒 + 𝐃𝑝, and the rate of Cauchy stress is given by 𝛔̇ = 𝐂𝐃𝑒. In out-of-plane compression the stress rate is modified according to 𝜎̇33 = 𝐶31𝐷11 𝑒 + 𝐶32𝐷22 𝑒 + 𝐷33 𝑒 { 𝑐 exp(−𝐶𝑐𝜀33 𝐸3 𝐸3, 𝑒 ) , 𝑒 ≥ 0, 𝜀33 𝑒 < 0. 𝜀33 For shell elements, 𝐷33 surface 𝑝 = 0, and only two yield surfaces are present: the in-plane yield 𝑓 = ∑ 𝑖=1 ⎡max(0, 𝜎: 𝑁𝑖) ⎢ 𝑓 ) 𝑞𝑖(𝜀𝑝 ⎣ 2𝑘 ⎤ ⎥ ⎦ − 1 ≤ 0 , and the transverse-shear yield surface ℎ = √𝜎13 2 + 𝜎23 𝜏0 + [𝐴𝜏 − min(0, 𝜎33) 𝐵𝜏]𝜀𝑝 − 1 ≤ 0, and the plastic flow rule is given by where the plastic velocity gradient is given as 𝛆̇𝑝 = 𝐃𝑝 = 𝐋𝑝, 𝐋𝑝 = 𝑓 𝜕𝑓 𝜕𝜎11 ⎡𝜀̇𝑝 ⎢ ⎢ 𝑓 𝜕𝑓 ⎢ 𝜀̇𝑝 ⎢ 𝜕𝜎12 ⎢ ⎢ ℎ 𝜕ℎ ⎢ 𝜀̇𝑝 𝜕𝜎13 ⎣ 𝑓 𝜕𝑓 𝜀̇𝑝 𝜕𝜎12 𝑓 𝜕𝑓 𝜀̇𝑝 𝜕𝜎22 ℎ 𝜕ℎ 𝜀̇𝑝 𝜕𝜎23 ℎ 𝜕ℎ 𝜀̇𝑝 𝜕𝜎13 ℎ 𝜕ℎ 𝜀̇𝑝 𝜕𝜎23 ⎤ ⎥ ⎥ ⎥ . ⎥ ⎥ ⎥ ⎥ ⎦ History variables: History variables 1 to 3 show 𝜀𝑝 𝑓 , 𝜀𝑝 𝑔 and 𝜀𝑝 ℎ, respectively. The Effective Plastic Strain is 𝑓 ) 𝜀𝑝 = √(𝜀𝑝 𝑔) + (𝜀𝑝 ℎ) + (𝜀𝑝 *MAT_SMOOTH_VISCOELASTIC_VISCOPLASTIC This is Material Type 275, a smooth viscoelastic viscoplastic model based on the works of Hollenstein et.al. [2013, 2014] and Jabareen [2015]. The stress response is rheologically represented by HJR (Hollenstein-Jabareen-Rubin) elements in parallel, see Figure 0-1, where each element exhibits combinations of viscoelastic and viscoplastic characteristics. The model is based on large displacement hyper-elastoplasticity and the numerical implementation is strongly objective, this together with the smooth characteristics makes it especially suitable for implicit analysis. Card 1 1 Variable MID 2 RO Type A8 F 3 K F 4 5 6 7 8 HJR Element Cards. At least 1 and optionally up to 6 cards should be input. A keyword card (with a “*” in column 1) terminates this input, if less than 6 cards are used. Card 2 Variable 1 A0 Type F 2 B0 F 3 A1 F 4 B1 F 5 M F 6 7 8 KAPAS KAPA0 SHEAR F F F VARIABLE MID DESCRIPTION Material identification. A unique number or label not exceeding 8 characters must be specified. RO K A0 B0 A1 B1 Mass density. Elastic bulk modulus. Rate dependent understress viscoplastic parameter. Rate independent understress plasticity parameter. Rate dependent overstress viscoplastic parameter. Rate independent overstress plasticity parameter. 𝐹 𝐺 𝑎0 𝑏0 𝑏1 𝑎1 𝜅(𝜅0, 𝜅𝑠, 𝑚) Figure 0-1. Rheological representation of an HJR element, including the associated parameters. VARIABLE DESCRIPTION Exponential hardening parameter. Saturated yield strain. Initial yield strain. Elastic shear modulus. M KAPAS KAPA0 SHEAR Remarks: The Cauchy stress for this smooth viscoelastic viscoplastic material is given by 𝛔 = 𝐾(𝐽 − 1)𝐈 + ∑ 𝐬𝑖 , 𝑖=1 where 𝐾 is the elastic bulk modulus provided on the first card, 𝐽 = det(𝐅) is the relative volume with 𝑭 being the total deformation gradient, and the deviatoric stresses 𝒔𝑖 are coming from the HJR (Hollenstein-Jabareen-Rubin) elements in parallel. Up to 6 such elements can be defined for the deviatoric response and a rheological representation of one is shown in Figure 0-1. Each element is associated with 8 material parameters that are provided on the optional cards and characterize its inelastic response. All this allows for a wide range of stress strain relationships and the critical part would be to estimate parameters for a given test suite, whence some elaboration on the physical interpretation of the individual parameters in the context of uniaxial stress is given following a general description of the model. We analyze one HJR element by letting 𝐁̅̅̅̅ denote the associated isochoric elastic left Cauchy-Green tensor. Define The evolution of 𝐁̅̅̅̅ is given by 𝐁̃ = 𝐁̅̅̅̅ − 1 3 𝛼𝐈, where 𝛼 = tr(𝐁̅̅̅̅ ). a0 = 0.0 a0 = 0.5 a0 = 1.0 a0 = 2.0 1.2 1.0 0.8 0.6 0.4 0.2 0.0 0.0 1.0 2.0 3.0 4.0 5.0 6.0 7.0 8.0 9.0 10.0 Time Figure M275-1. Influence of parameter 𝑎0 on stress relaxation 𝐁̅̅̅̅̇ = 𝐋𝐁̅̅̅̅ + 𝐁̅̅̅̅ 𝐋T − tr(𝐃)𝐁̅̅̅̅ − 𝛤̇𝐀, where 𝐀 = 𝐁̅̅̅̅ − [ tr(𝐁̅̅̅̅ −1) ] 𝐈 where 𝐃 is the rate-of-deformation and 𝛤̇ governs the inelastic deformation. The functional form of 𝛤̇ is summarized in the following set of equations where 𝛤̇ = 𝛤̇0 + ⟨𝑔⟩𝛤̇1 𝛤̇𝑖 = 𝑎𝑖 + 𝑏𝑖𝜀̇, 𝑔 = 1 − 𝛾̃ 𝑖 = 0,1 ⟨𝑔⟩ = max(0, 𝑔) , 𝜀̇ = √ 𝐃̃ ∶ 𝐃̃ , 𝐃̃ = 𝐃 − tr(𝐃)𝐈, 𝛾̃ = √ 𝐁̃ ∶ 𝐁̃ , 𝜅̇ = 𝑚𝛤̇1⟨𝑔⟩(𝜅𝑠 − 𝜅). A hyperelastic law with a strain energy potential for the distortional deformation given by b0 = 0 b0 = 5 b0 = 25 b0 = 50 0.300 0.200 0.100 0.000 -0.100 -0.200 -0.300 -15.0 -10.0 -5.0 0.0 5.0 10.0 15.0 Strain % Figure M275-2. Influence of 𝑏0 in cyclic loading 𝜓(𝛼) = (𝛼 − 3) yields a contribution to the deviatoric Cauchy stress of 𝐬 = 𝐺𝐽−1𝐁̃ . In uniaxial stress at constant total distortional rate of deformation ±𝜀̇ (tension or compression), these equations can be reduced to scalar correspondents 𝑏̅ 𝑏̅ = 2 ⎜⎜⎛±𝜀̇ − 𝛤̇ ⎝ 𝑏̅√𝑏̅ − 1 ⎟⎟⎞ 2𝑏̅√𝑏̅ + 1⎠ 𝜏 = 𝐺 ⎜⎛𝑏̅ − ⎝ ⎟⎞ √𝑏̅⎠ (M275.1) where 𝑏̅ is the component of 𝑩̅̅̅̅̅ in the direction of deformation and 𝜏 is the uniaxial Kirchhoff stress. The evolution of 𝛤 follows the equations above with 𝛾̃ = 1 2 ∣𝑏̅ − 1/√𝑏̅∣. Even though analytical solutions may be out of reach, this would be the basis for estimating as well as interpreting the material parameters. Obviously the shear modulus 𝐺 (SHEAR) provides the elastic deviatoric stiffness, for a purely elastic material just define one such parameter and leave out all the other parameters on the same card. If several cards are used, the effective elastic shear stiffness is the sum of the 2-1404 (MAT_248) 0.07 0.05 0.02 0.00 -0.03 -0.05 -0.08 b1 = 100 b1 = 200 b1 = 500 b1 = 1000 0.0 0.5 1.0 1.5 2.0 2.5 3.0 3.5 4.0 4.5 5.0 Strain % Figure M275-3. Effect of 𝑏1 in cyclic loading contributions from each of the corresponding HJR elements. An interesting observation is that the stress in a HJR element saturates to a value given by the solution of 𝑏̅ to 𝑏̅√𝑏̅ (±2 − {𝑏0 + 𝑏1 + 𝑎0 + 𝑎1 𝜀̇ }) ± 2√𝑏̅𝜅𝑠 (𝑏1 + ) 𝑎1 𝜀̇ 𝑎0 + 𝑎1 𝜀̇ + (±1 + {𝑏0 + 𝑏1 + }) = 0 (M275.2) in tension (+) and compression (−), followed by application of (M275.1) above, this assuming that in tension 𝑏0 + 𝑏1 + 𝑎0 + 𝑎1 𝜀̇ > 2 𝑏0 + 𝑏1 + 𝑎0 + 𝑎1 𝜀̇ > 1 in compression. This expression will be utilized in special cases below when examining each inelastic material parameter individually, the material parameters above are input on the HJR element cards as A0, B0, A1, B1 and KAPAS. A Maxwell material is obtained by providing an element with a nonzero 𝑎0 (A0) and other parameters zero, this parameter should be interpreted as the viscoelastic relaxation coefficient determining the rate at which the stress relaxes to zero, see parameter BETA in *MAT_VISCOELASTIC. In Figure M275-1 a stress relaxation is shown for a strain controlled problem using two HJR elements and normalized material parameters using a bulk modulus of 𝐾 = 1. For the first element 𝐺 = 0.5 and for the other 𝐺 = 1 and 𝑎0 varies, all other parameters are zero. The engineering strain is ramped to 50% from 𝑡 = 0 to 𝑡 = 1 and then kept constant, the response is very similar to other viscoelastic models in LS-DYNA. Not surprisingly, a HJR element with 𝑎0 > 0 (and 𝑎1 = 𝑏1 = 0) will always relax to zero stress, which follows from (M275.1) and (M275.2), thus the relaxed stress in this case comes from the purely elastic element. A general viscoelastic material can be obtained by putting several such HJR elements in parallel, in analogy to *MAT_GENERAL_VISCOELASTIC. For a nonzero 𝑏0 (B0) and other parameters zero, a rate independent plastic response is obtained exhibiting zero yield stress, i.e., inelastic strains develop immediately upon loading. From (M275.2) the value of 𝑏0 determines the saturated stress value for the associated HJR element by (M275.1) and 𝑏̅ = ( 𝑏0 ± 1 𝑏0 ∓ 2 2/3 ) in tension (+) and compression (−), respectively. A smooth response is obtained that is characterized by hysteresis as shown in Figure M275-2. The same material parameters as in the previous example is used with the exception of varying 𝑏0 with vanishing 𝑎0. The deformation is controlled by a cyclic Cauchy stress between −0.25 and 0.25, for larger 𝑏0 a hysteresis is observed. It should however be mentioned that the hysteresis vanishes as 𝑏0 → ∞ as the stress for the second element saturates quickly to a small value, so it is not trivial to quantitatively estimate the amount of hysteresis for a given parameter setting and deformation. 0.07 0.05 0.02 0.00 -0.03 -0.05 -0.08 m = 0.1 m = 0.2 m = 0.5 m = 1.0 0.0 0.5 1.0 1.5 2.0 2.5 3.0 3.5 4.0 4.5 5.0 Strain % Figure M275-4. Softening response in cyclic loading for various values of 𝑚 Rate independent plasticity with a nonzero yield stress can be obtained by a nonzero 𝑏1 (B1) in combination with parameters 𝜅0 (KAPA0), 𝜅𝑠 (KAPAS) and 𝑚 (M). The yield stress in the sense of von Mises is given by 𝜎𝑌 = 2𝐺𝐽−1𝜅 and whence 𝜅 is interpreted as the current yield strain. Here 𝑏1 determines the amount of overstress through (M275.1) and (M275.2), requiring the solution of a non-trivial polynomial equation. This is exemplified in Figure M275-3 using one HJR element with 𝐾 = 1, 𝐺 = 1.5, 𝜅0 = 𝜅𝑠 = 0.01 and 𝑚 = 0. The engineering strain is ramped up to 5% and down to 0 and 𝑏1 is varied with all other parameters zero, the response tends to an elastic-perfectly plastic as 𝑏1 increases. The saturated stress value for 𝑏1 → ∞ can be calculated as 𝑏̅ = ⎡ ⎜⎜⎛1 ⎢⎢ ⎝ ⎣ + √ ∓ 8𝜅𝑠 27 ⎟⎟⎞ ⎠ 1/3 + ⎜⎜⎛1 ⎝ − √ ∓ 8𝜅𝑠 27 ⎟⎟⎞ ⎠ 1/3 ⎤ ⎥⎥ ⎦ (M275.3) and employing (M275.1). Isostropic strain hardening 𝜅𝑠 > 𝜅0 or softening 𝜅𝑠 < 𝜅0 is obtained with 𝑚 > 0, 𝜅 tends exponentially towards 𝜅𝑠 at a rate determined by 𝑚. Using 𝑏1 = 1000, i.e., very little overstress, 𝜅0 = 0.02, 𝜅𝑠 = 0.01 and varying 𝑚 the softening response in Figure M275-4 is obtained. The rate at which the element hardens is difficult to quantitatively estimate, but presumably it depends not only on 𝑚 but also on 𝑏1. It is important to note however that for small to moderate 𝑏1 the model appears to harden with 𝑚 = 0, de/dt = 0.2 de/dt = 4.0 de/dt = 10.0 de/dt = 20.0 0.125 0.100 0.075 0.050 0.025 0.000 -0.025 -0.050 -0.075 0.0 0.5 1.0 1.5 2.0 2.5 3.0 3.5 4.0 4.5 5.0 Strain % Figure M275-5. Strain rate dependence for 𝑎1 = 1000 and 𝑏1 = 10 which is due to larger overstress. The hardening determined by 𝑚 can be determined from a loading, unloading and reloading cycle to detect how the the yield strain 𝜅 changes, see Hollenstein et.al. [2013]. Finally, 𝑎1 (A1) is the viscoplastic parameter determining how stress responds to change in strain rate. Its interpretation is very similar to that of 𝑎0, stress increases with increasing loading rate and relaxes to the saturated stress value given by (M275.1) and (M275.2). In Figure M275-5 a rate dependency is illustrated for 𝐾 = 1, 𝐺 = 1.5, 𝜅0 = 𝜅𝑠 = 0.01 and 𝑚 = 0, where we have put 𝑎1 = 1000 and 𝑏1 = 10. The engineering strain rate varies from 0.2 to 20 and for small strain rates (M275.3) can be used for estimating the saturated stress, but in general (M275.2) must be used. Putting several HJR elements in parallel can thus provide a fairly general combination of viscoelastic/viscoplastic response with isotropic hardening/softening, but this of course requires a rich test suite and a good way of estimating the material parameters. Presumably it is often sufficient to neglect some effects and work with only a subset of the material parameters. For post-processing, the effective plastic strain in this model is defined as where 𝜀𝑝 = √ 𝛆𝑝 ∶ 𝛆𝑝 𝛆𝑝 = 𝛆𝑡 − 𝛆𝑒 is a crude estimation of the difference between total and elastic strain. We set where 𝛆𝑡 = 2𝐽 [𝐁 − tr(𝐁)𝐈] 𝛆𝑒 = 2𝐺 [𝛔 − tr(σ)𝐈] 𝐁 = 𝐽−2/3𝐅𝐅T and 𝐺 here is the sum of all shear moduli defined on the HJR element cards. Note that this does not correspond to the traditional measure of effective plastic strain which should be accounted for when validating results. *MAT_CHRONOLOGICAL_VISCOELASTIC This is Material Type 276. This material model provides a general viscoelastic Maxwell model having up to 6 terms in the prony series expansion and is useful for modeling dense continuum rubbers and solid explosives. It is similar to Material Type 76 but allows the incorporation of aging effects on the material properties. Either the coefficients of the prony series expansion or a relaxation curve may be specified to define the viscoelastic deviatoric and bulk behavior. The material model can also be used with laminated shell. Either an elastic or viscoelastic layer can be defined with the laminated formulation. To activate laminated shell you need the laminated formulation flag on *CONTROL_SHELL. With the laminated option a user defined integration rule is needed. Card 1 1 Variable MID 2 RO 3 4 BULK PCF Type A8 F F F 5 EF F 6 TREF F 7 A F 8 B F If fitting is done from a relaxation curve, specify fitting parameters on card 2, otherwise if constants are set on Viscoelastic Constant Cards LEAVE THIS CARD BLANK. Card 2 1 2 3 4 5 6 7 8 Variable LCID NT BSTART TRAMP LCIDK NTK BSTARTK TRAMPK Type F I F F F I F Viscoelastic Constant Cards. Up to 12 cards may be input. A keyword card (with a “*” in column 1) terminates this input if less than 12 cards are used. These cards are not needed if relaxation data is defined. The number of terms for the shear behavior may differ from that for the bulk behavior: simply insert zero if a term is not included. If an elastic layer is defined you only need to define GI and KI (note in an elastic layer only one card is needed). Optional Variable Type 1 GI F 2 BETAI F 3 KI F VARIABLE MID 4 5 6 7 8 BETAKI F DESCRIPTION Material identification. A unique number or label not exceeding 8 characters must be specified. RO Mass density. BULK Elastic bulk modulus. PCF EF TREF A B LCID NT Tensile pressure elimination flag for solid elements only. If set to unity tensile pressures are set to zero. Elastic flag (if equal 1, the layer is elastic. If 0 the layer is viscoelastic). Reference temperature for shift function (must be greater than zero). Chronological coefficient 𝛼(𝑡𝑎). See Remarks below. Chronological coefficient 𝛽(𝑡𝑎). See Remarks below. Load curve ID for deviatoric behavior if constants, Gi, and βi are determined via a least squares fit. This relaxation curve is shown below. Number of terms in shear fit. If zero the default is 6. Fewer than NT terms will be used if the fit produces one or more negative shear moduli. Currently, the maximum number is set to 6. BSTART *MAT_CHRONOLOGICAL_VISCOELASTIC DESCRIPTION In the fit, 𝛽1 is set to zero, 𝛽2 is set to BSTART, 𝛽3 is 10 times 𝛽2, 𝛽4 is 10 times 𝛽3 , and so on. If zero, BSTART is determined by an iterative trial and error scheme. TRAMP Optional ramp time for loading. LCIDK Load curve ID for bulk behavior if constants, 𝐾𝑖, and 𝛽𝐾𝑖 are determined via a least squares fit. This relaxation curve is shown below. NTK Number of terms desired in bulk fit. If zero the default is 6. Currently, the maximum number is set to 6. BSTARTK In the fit, Β𝐾1 is set to zero, Β𝐾2 is set to BSTARTK, 𝛽𝐾3 is 10 times 𝛽𝐾2, is 𝛽𝐾4 10 times 𝛽𝐾3 , and so on. If zero, BSTARTK is determined by an iterative trial and error scheme. TRAMPK Optional ramp time for bulk loading. Gi Optional shear relaxation modulus for the ith term BETAi Optional shear decay constant for the ith term Ki Optional bulk relaxation modulus for the ith term BETAKi Optional bulk decay constant for the ith term Remarks: The Cauchy stress, 𝜎𝑖𝑗, is related to the strain rate by 𝜎𝑖𝑗(𝑡) = −𝑝𝛿𝑖𝑗 + ∫ 𝑔𝑖𝑗𝑘𝑙(𝑡 − 𝜏) ∂𝜀𝑘𝑙(𝜏) ∂𝜏 𝑑𝜏 For this model, it is postulated that the mathematical form is preserved in the ′ (𝑡𝑎, 𝑡) constitutive equation for aging; however two new material functions, 𝑔0 are introduced to replace 𝑔0 and 𝑔1(𝑡), which is expressed in terms of a Prony series as in material model 76, *MAT_GENERAL_VISCOELASTIC. The aging time is denoted by 𝑡𝑎. ′ (𝑡𝑎) and 𝑔1 𝜎𝑖𝑗(𝑡𝑎, 𝑡) = −𝑝𝛿𝑖𝑗 + ∫ 𝑔𝑖𝑗𝑘𝑙 ′ (𝑡𝑎, 𝑡 − 𝜏) ∂𝜀𝑘𝑙(𝜏) ∂𝜏 𝑑𝜏 where ′ (𝑡𝑎, 𝑡) = 𝛼(𝑡𝑎)𝑔𝑖𝑗𝑘𝑙[𝛽(𝑡𝑎)𝑡] 𝑔𝑖𝑗𝑘𝑙 where 𝛼(𝑡𝑎) and 𝛽(𝑡𝑎) are two new material properties that are functions of the aging time 𝑡𝑎. The material properties functions 𝛼(𝑡𝑎) and 𝛽(𝑡𝑎) will be determined with the experimental results. For determination of 𝛼(𝑡𝑎) and 𝛽(𝑡𝑎), Eq. (2) can be written in the following form log(𝜎𝑖𝑗 − 𝑝𝛿𝑖𝑗) = log𝛼(𝑡𝑎) + log(𝜎𝑖𝑗 − 𝑝𝛿𝑖𝑗) 𝑡𝑎=0,𝑡→𝜉 𝑡𝑎,𝑡 log𝜉 = log𝛽(𝑡𝑎) + log𝑡 Therefore, if one plots the stress versus time on log-log scales, with the vertical axis being the stress and the horizontal axis being the time, then the stress-relaxation curve for any aged time history can be obtained directly from the stress-relaxation curve at 𝑡𝑎 = 0 by imposing a vertical shift and a horizontal shift on the stress-relaxation curves. The vertical shift and the horizontal shift are log𝛼(𝑡𝑎) and log𝛽(𝑡𝑎) respectively. *MAT_ADHESIVE_CURING_VISCOELASTIC This is Material Type 277. It is useful for modeling adhesive materials during chemical curing. This material model provides a general viscoelastic Maxwell model having up to 16 terms in the Prony series expansion. It is similar to Material Type 76, but the viscoelastic properties do not only depend on the temperature but also on an internal variable representing the state of cure for the adhesive. The kinematic of the curing process depends on temperature as well as on temperature rate and follows the Kamal model. Card 1 1 Variable MID Type A8 Card 2 1 2 RO F 2 3 K1 F 3 4 K2 F 4 5 C1 F 5 Variable CHEXP1 CHEXP2 CHEXP3 LCCHEXP LCTHEXP Type F Card 3 1 F 2 F 3 I 4 I 5 6 C2 F 6 R F 6 7 M F 7 8 N F 8 TREFEXP DOCREFE XP F 7 F 8 Variable WLFTREF WLFA WLFB LCG0 LCK0 IDOC INCR Type F F F I I F I Viscoelastic Constant Cards. Up to 16 cards may be input. A keyword card (with a “*” in column 1) terminates this input if less than 16 cards are used. The number of terms for the shear behavior may differ from that for the bulk behavior: simply insert zero if a term is not included. Optional Variable Type 1 GI F 2-1414 (MAT_248) 2 BETAGI F 3 KI F 4 5 6 7 8 BETAKI VARIABLE MID DESCRIPTION Material identification. A unique number or label not exceeding 8 characters must be specified. RO K1 K2 C1 C2 M N Mass density. Parameter 𝑘1 for Kamal model. Parameter 𝑘2 for Kamal model. Parameter 𝑐1 for Kamal model. Parameter 𝑐2 for Kamal model. Exponent 𝑚 for Kamal model Exponent 𝑛 for Kamal model. CHEXP1 CHEXP2 CHEXP3 LCCHEXP LCTHEXP R TREFEXP DOCREFEXP Quadratic parameter 𝛾2 for chemical shrinkage. Linear parameter 𝛾1 for chemical shrinkage. Constant parameter 𝛾0 for chemical shrinkage. Load curve ID to define the coefficient for chemical shrinkage 𝛾(𝛼) as a function of the state of cure 𝛼. If set, parameters CHEXP1, CHEXP2 and CHEXP3 are ignored. Load curve ID or table ID defining the instantaneous coefficient of thermal expansion 𝛽(𝛼, 𝑇) as a function of cure 𝛼 and temperature 𝑇. If referring to a load curve, parameter 𝛽(𝑇) is a function of temperature 𝑇. Gas constant 𝑅 for Kamal model. Reference temperature 𝑇0 for secant form of thermal expansion. See Remarks below. Reference degree of cure 𝛼0 for sequential form of chemical expansion. See Remarks below. WLFTREF Reference temperature for WLF shift function. WLFA WLFB Parameter 𝐴 for WLF shift function. Parameter 𝐵 for WLF shift function. *MAT_ADHESIVE_CURING_VISCOELASTIC DESCRIPTION LCG0 LCK0 IDOC INCR Load curve ID defining the instantaneous shear modulus 𝐺0 as a function of state of cure. Load curve ID defining the instantaneous bulk modulus 𝐾0 as a function of state of cure. Initial degree of cure. Switch between incremental and total stress formulation. EQ.0: total form: (DEFAULT) EQ.1: incremental form: (recommended) GI Shear relaxation modulus for the ith term for fully cured material. BETAGI Shear decay constant for the ith term for fully cured material. KI Bulk relaxation modulus for the ith term for fully cured material. BETAKI Bulk decay constant for the ith term for fully cured material. Remarks: Within this material formulation an internal variable 𝛼 has been included to represent the degree of cure for the adhesive. The evolution equation for this variable is given by the Kamal model and reads dα dt = (𝑘1 exp ( −𝑐1 𝑅𝑇 ) + 𝑘2 exp ( −𝑐2 𝑅𝑇 ) 𝛼𝑚) (1 − 𝛼)𝑛 The chemical reaction of the curing process results in a shrinkage of the material. The coefficient of the chemical shrinkage 𝛾(𝛼) can either be given by a load curve or using the quadratic expression 𝛾(𝛼) = 𝛾2𝛼2 + 𝛾1𝛼 + 𝛾0 For non-negative values of the reference degree of cure 𝛼0, a secant form is used to compute the chemical strains Otherwise a differential form is used: 𝜀𝑐ℎ = 𝛾(𝛼)(𝛼 − 𝛼0) − 𝛾(𝛼𝐼)(𝛼𝐼 − 𝛼0) 𝑑𝜀𝑐ℎ = 𝛾(𝛼)𝑑𝛼 Analogously, the thermal strains are either defined in a secant or differential form, depending on the reference temperature 𝑇0. In both cases the coefficient of thermal expansion can be given as 2d table depending on degree of cure and temperature. Finally, the Cauchy stress, 𝜎𝑖𝑗, is related to the strain rate by 𝜎𝑖𝑗(𝑡) = ∫ 𝑔𝑖𝑗𝑘𝑙(𝑡 − 𝜏) ∂𝜀𝑘𝑙(𝜏) ∂𝜏 𝑑𝜏 The relaxation functions 𝑔𝑖𝑗𝑘𝑙(𝑡 − 𝜏) are represented in this material formulation by up to 16 terms (not including the instantaneous modulus 𝐺0) of the Prony series: g(𝑡, 𝛼) = 𝐺0(𝛼) − ∑ 𝐺𝑖(𝛼) + ∑ 𝐺𝑖(𝛼) 𝑒−𝛽𝑖𝑡 For the sake of simplicity, a constant ratio 𝐺𝑖(𝛼) 𝐺0(𝛼) for all degrees of cure is assumed. Consequently, it suffices to define one term 𝐺0(𝛼) as a function of the degree of cure and further coefficients for the fully cured state of the adhesive: ⁄ g(𝑡, 𝛼) = 𝐺0(𝛼) ⎜⎜⎛1 − ∑ ⎝ 𝐺𝑖,𝛼=1.0 𝐺0,𝛼=1.0 (1 − 𝑒−𝛽𝑖𝑡) ⎟⎟⎞ ⎠ A possible temperature effect on the stress relaxation is accounted for by the Williams- Landau-Ferry (WLF) shift function. For details on this function, please see material formulation 76, *MAT_GENERAL_VISCOELASTIC. *MAT_CF_MICROMECHANICS This is Material Type 278 developed for draping and curing analysis of prepreg carbon fiber sheets. This material model is mixture of MAT_234 and MAT_277, with MAT_234 providing reorientation and locking phenomenon of fibers and MAT_277 providing the viscoelastic behavior of epoxy resin. The overall stress has contribution from both fiber orientation and deformation and epoxy resin. Card 1 1 Variable MID Type A8 Card 2 1 2 RO F 2 3 E1 F 3 4 E2 F 4 5 6 G12 G23 F 5 Variable EKA EUA VMB EKB THL Type F Card 3 Variable Type 1 W F F 2 F 3 SPAN THICK F F Card 4 1 Variable AOPT Type 2 A1 F 3 A2 F F 4 H F 4 A3 F F 5 AREA F 5 7 EU F 7 8 C F 8 THI1 THI2 F 7 F 8 F 6 TA F 6 6 7 Variable 1 V1 Type F 2 V2 F 3 V3 F 4 D1 F 5 D2 F 6 D3 F *MAT_278 7 8 Card 6 1 2 3 4 5 6 7 8 Variable VYARN Type F Card 6 Variable 1 K1 Type F 2 K2 F 3 C1 F 4 C2 F 5 M F Card 7 1 2 3 4 5 Variable EXP1 CHEXP2 CHEXP3 LCCHEX LCTHEXP0 Type F Card 8 1 F 2 F 3 F 4 F 5 6 N F 6 R F 6 7 8 7 8 TREFEXP ALPREEXP F 7 F 8 Variable WLFTREF WLFA WLFB LCG0 LCBULK0 IDOC XINCRM Type F F F F F F Viscoelastic Constant Cards. Up to 14 cards may be input. A keyword card (with a “*” in column 1) terminates this input if less than 14 cards are used. The number of terms for the shear behavior may differ from that for the bulk behavior: simply insert zero if a term is not included. Card 8 Variable Type 1 GI F 2 BETAGI F 3 KI F 4 5 6 7 8 BETAKI F VARIABLE DESCRIPTION MID RO E1 E2 G12 G23 EU C EKA EUA VMB Ekb THL TA THI1 THI2 W SPAN THICK H Material identification. A unique number or label not exceeding 8 characters must be specified. Mass density. 𝐸1, Young’s modulus in the yarn axial-direction. 𝐸2, Young’s modulus in the yarn transverse-direction. 𝐺12, Shear modulus of the yarns. transverse shear modulus. Ultimate strain at failure. Coefficient of friction between the fibers. Elastic constant of element "a". Ultimate strain of element "a". Damping coefficient of element "b". Elastic constant of element "b" Yarn locking angle. Transition angle to locking. Initial braid angle 1. Initial braid angle 2. Fiber width. Span between the fibers. Real fiber thickness. Effective fiber thickness. VARIABLE DESCRIPTION AREA APOT VYARN K1 K2 C1 C2 M N CHEXP1 CHEXP2 CHEXP3 LCCHEXP LCTHEXP R TREFEXP DOCREFEXP Fiber cross-sectional area. Material axes option . Volume fraction of yarn Parameter 𝑘1 for Kamal model. Parameter 𝑘2 for Kamal model. Parameter 𝑐1 for Kamal model. Parameter 𝑐2 for Kamal model. Exponent 𝑚 for Kamal model Exponent 𝑛 for Kamal model. Quadratic parameter 𝛾2 for chemical shrinkage. Linear parameter 𝛾1 for chemical shrinkage. Constant parameter 𝛾0 for chemical shrinkage. Load curve ID to define the coefficient for chemical shrinkage 𝛾(𝛼) as a function of the state of cure 𝛼. If set, parameters CHEXP1, CHEXP2 and CHEXP3 are ignored. Load curve ID or table ID defining the instantaneous coefficient of thermal expansion 𝛽(𝛼, 𝑇) as a function of cure 𝛼 and temperature 𝑇. If referring to a load curve, parameter 𝛽(𝑇) is a function of temperature 𝑇. Gas constant 𝑅 for Kamal model. Reference temperature 𝑇0 for secant form of thermal expansion. Reference degree of cure 𝛼0 for sequential form of chemical expansion. WLFTREF Reference temperature for WLF shift function. WLFA WLFB LCG0 LCK0 Parameter 𝐴 for WLF shift function. Parameter 𝐵 for WLF shift function. Load curve ID defining the instantaneous shear modulus 𝐺0 as a function of state of cure. Load curve ID defining the instantaneous bulk modulus 𝐾0 as a function of state of cure. IDOC Initial degree of cure. *MAT_CF_MICROMECHANICS DESCRIPTION INCR Switch between incremental and total stress formulation. EQ.0: total form: (DEFAULT) EQ.1: incremental form: (recommended) GI Shear relaxation modulus for the ith term for fully cured material. BETAGI Shear decay constant for the ith term for fully cured material. KI Bulk relaxation modulus for the ith term for fully cured material. BETAKI Bulk decay constant for the ith term for fully cured material. *MAT_279 This is material type 279. This is a cohesive model for paper materials and can be used only with cohesive element fomulations; see the variable ELFORM in *SECTION_SOL- ID and *SECTION_SHELL. Card 1 1 2 3 4 5 6 7 8 Variable MID RO ROFLG INTFAIL EN0 ET0 EN1 ET1 Type A8 F F F F F F F Default none none none none none none none none Card 2 1 Variable T0N 2 DN 3 4 T1N T0T Type F F F F 5 DT F 6 7 T1T E3C F F 8 CC F Default none none none none none none none none Card 3 1 2 3 4 5 6 7 8 Variable ASIG BSIG CSIG FAILN FAILT Type F F F F F Default none none none none none VARIABLE MID DESCRIPTION Material identification. A unique number or label not exceeding 8 characters must be specified. RO Mass density ROFLG Flag for whether density is specified per unit area or volume. ROFLG.EQ.0: specified density per unit volume (default) ROFLG.EQ.1: specifies the density is per unit area for controlling the mass of cohesive elements with an initial volume of zero. INTFAIL The number of integration points required for the cohesive element to be deleted. If it is zero, the element will not be deleted even if it satisfies the failure criterion. The value of INTFAIL may range from 1 to 4, with 1 the recommended value. EN0 EN1 ET0 ET1 T0N DN T1N T0T DT T1T E3C CC ASIG BSIG The initial tensile stiffness (units of stress / length) normal to the plane of the cohesive element. The final tensile stiffness (units of stress / length) normal to the plane of the cohesive element. The initial stiffness (units of stress / length) tangential to the plane of the cohesive element. The final stiffness (units of stress / length) tangential to the plane of the cohesive element. Peak tensile traction in normal direction. Scale factor (unit of length). Final tensile traction in normal direction. Peak tensile traction in tangential direction. If negative, the absolute value indicates a curve with respect to the normal traction. Scale factor (unit of length). If negative, the absolute value indicates a curve with respect to the normal stress. Final traction in tangential direction. If negative, the absolute value indicates a curve with respect to the normal traction. Elastic parameter in normal compression. Elastic parameter in normal compression. Plasticity hardening parameter in normal compression. Plasticity hardening parameter in normal compression. 𝑇 𝑇0 𝐸0 𝐸(𝛿 ̅ 𝑝) 𝑇1 Figure M279-1. Traction-separation law CSIG Plasticity hardening parameter in normal compression. Maximum effective separation distance in normal direction. Beyond this distance failure occurs. Maximum effective separation distance in tangential direction. Beyond this distance failure occurs. FAILN FAILT Remarks: In this elastoplastic cohesive material the normal and tangential directions are treated separately, but can be connected by expressing the in-plane traction parameters as functions of the normal traction. In the normal direction the material uses different models in tension and compression. Normal tension: Assume the total separation is an additive split of the elastic and plastic separation 𝛿 = 𝛿𝑒 + 𝛿𝑝 . In normal tension (𝛿𝑒 > 0) the elastic traction is given by 𝑇 = 𝐸𝛿𝑒 = 𝐸(𝛿 − 𝛿𝑝) ≥ 0, where the tensile normal stiffness 𝐸 = (𝐸𝑁 0 − 𝐸𝑁 1 ) exp −𝛿 ̅ 𝛿𝑁 ⎠ ⎟⎞ + 𝐸𝑁 1 , ⎜⎛ ⎝ depends on the effective plastic separation in the normal direction Yield traction for tensile loads in normal direction is given by 𝛿 ̅ 𝑝 = ∫∣d𝛿𝑝∣ . 𝑇yield = (𝑇𝑁 0 − 𝑇𝑁 1 ) exp ⎜⎛ ⎝ −𝛿 ̅ 𝛿𝑁 ⎠ ⎟⎞ + 𝑇𝑁 1 ≥ 0, and yielding occurs when 𝑇 > 𝑇yield ≥ 0. The above elastoplastic model gives the traction-separation law depicted in Figure M279-1. Normal compression: In normal compression the elastic traction is and the yield traction is 𝑇 = 𝐸3 𝑐 [1 − exp(−𝐶𝑐𝛿𝑒)] ≤ 0, 𝑇yield = −[𝐴𝜎 + 𝐵𝜎 exp(−𝐶𝜎𝛿 ̅ 𝑝)] ≤ 0, with yielding if 𝑇 < 𝑇yield ≤ 0. Tangential traction: Assume the total separation is an additive split of the elastic and plastic separation in each in-plane direction The elastic traction is given by 𝛿𝑖 = 𝛿𝑒 𝑖 , 𝑖 + 𝛿𝑝 𝑖 = 1,2. where the tensile normal stiffness 𝑇𝑖 = 𝐸𝛿𝑒 𝑖 = 𝐸(𝛿𝑖 − 𝛿𝑝 𝑖 ), 𝐸 = (𝐸𝑇 0 − 𝐸𝑇 1 ) exp −𝛿 ̅ 𝛿𝑇 ⎠ ⎟⎞ + 𝐸𝑇 1 , ⎜⎛ ⎝ depends on the effective plastic separation 𝛿 ̅ 𝑝 = ∫ d𝛿𝑝 , d𝛿𝑝 = √(d𝛿𝑝 1) 2) + (d𝛿𝑝 . Yield traction is given by 𝑇yield = (𝑇𝑇 0 − 𝑇𝑇 ⎜⎛ 1 ) exp ⎝ −𝛿 ̅ 𝛿𝑇 ⎠ ⎟⎞ + 𝑇𝑇 1 , and yielding occurs when 2 + 𝑇2 𝑇1 2 − 𝑇𝑦𝑖𝑒𝑙𝑑 2 ≥ 0. The plastic flow increment follows the flow rule d𝛿𝑝 𝑖 = 𝑇𝑖 2 + 𝑇2 √𝑇1 d𝛿𝑝. The above elastoplastic model gives the traction-separation law depicted in Figure M279-1. History variables This material uses five history variables. Effective separation in the tangential direction is saved as Effective Plastic Strain. History variable 1 and 2 indicates the plastic separation in each tangential direction. Effective plastic separation and plastic separation in the normal direction are saved as history variable 3 and 4, respectively. *MAT_GLASS This is Material Type 280. It is a smeared fixed crack model with a selection of different brittle, stress-state dependent failure criteria such as Rankine, Mohr-Coulomb, or Drucker-Prager. The model incorporates up to 2 (orthogonal) cracks per integration point, simultaneous failure over element thickness, and crack closure effects. It is available for shell elements and explicit analysis only. Card 1 1 Variable MID 2 RO Type A8 F Card 2 1 Variable FMOD Type F Card 3 1 2 FT F 2 3 E F 3 FC F 3 4 PR F 4 AT F 4 5 6 7 8 IMOD ILAW F 7 BC F 7 F 8 8 5 BT F 5 6 AC F 6 Variable SFSTI SFSTR CRIN ECRCL NCYCR NIPF Type F F F F F F VARIABLE DESCRIPTION MID RO E PR Material identification. A unique number or label not exceeding 8 characters must be specified. Mass density 𝜌. Young’s modulus 𝐸. Poisson’s ratio 𝜈. IMOD *MAT_280 DESCRIPTION Flag to choose degradation procedure, when critical stress is reached. EQ.0.0: Softening in NCYCR load steps. Define SFSTI, SFSTR, and NCYCR (default). EQ.1.0: Damage model for softening. Define ILAW, AT, BT, AC, and BC. ILAW Flag to choose damage evolution law if IMOD = 1.0, see Remarks. EQ.0.0: Same damage evolution for tensile and compressive failure (default). EQ.1.0: Different damage evolution for tensile failure and compressive failure. FMOD Flag to choose between failure criteria, see Remarks. EQ.0.0: Rankine maximum stress (default), EQ.1.0: Mohr-Coulomb, EQ.2.0: Drucker-Prager. Tensile strength 𝑓𝑡. Compressive strength 𝑓𝑐. Tensile damage evolution parameter 𝛼𝑡. Can be interpreted as the residual load carrying capacity ratio for tensile failure ranging from 0 to 1. Tensile damage evolution parameter 𝛽𝑡. It controls the softening velocity for tensile failure. Compressive damage evolution parameter 𝛼𝑡. Can be interpreted as the residual load carrying capacity ratio for compressive failure ranging from 0 to 1. Compressive damage evolution parameter 𝛽𝑡. It controls the softening velocity for compressive failure. Scale factor for stiffness after failure, e.g. SFSTI = 0.001 means that stiffness is reduced to 0.1% of the elastic stiffness at failure. Scale factor for stress in case of failure, e.g. SFSTR = 0.01 means that stress is reduced to 1% of the failure stress at failure. FT FC AT BT AC BC SFSTI SFSTR *MAT_GLASS DESCRIPTION ICRIN Flag for crack strain initialization EQ.0.0: initial crack strain is strain at failure (default), EQ.1.0: initial crack strain is zero. Crack strain necessary to reactivate certain stress components after crack closure. Number of cycles in which the stress is reduced to SFSTR*failure stress. Number of failed through thickness integration points to fail all through thickness integration points for IMOD = 0. ECRCL NCYCR NIPF Remarks: The underlying material behavior before failure is isotropic, small strain linear elasticity with Young’s modulus 𝐸 and Poisson’s ratio 𝜈. Asymmetric (tension-compression dependent) failure happens as soon as one of the following plane stress failure criteria is violated. For FMOD = 0, a maximum stress criterion (Rankine) is used, where principal stresses 𝜎1 and 𝜎2 are bound by tensile strength 𝑓𝑡 and compressive strength 𝑓𝑐 as follows: −𝑓𝑐 < {𝜎1, 𝜎2} < 𝑓𝑡 With FMOD = 1, the Mohr-Coulomb criterion with expressions in four different categories is used: 𝜎1 > 0 and 𝜎2 > 0: max ( 𝜎1 < 0 and 𝜎2 < 0: max (− 𝜎1 𝑓𝑡 𝜎1 𝑓𝑐 , 𝜎2 𝑓𝑡 ) < 1 , − 𝜎2 𝑓𝑐 ) < 1 𝜎1 > 0 and 𝜎2 < 0: − < 1 𝜎1 < 0 and 𝜎2 > 0: − + < 1 𝜎1 𝑓𝑡 𝜎1 𝑓𝑐 𝜎2 𝑓𝑐 𝜎2 𝑓𝑡 And for FMOD = 2, the plane stress Drucker-Prager criterion is given by 2𝑓𝑐 [( 𝑓𝑐 𝑓𝑡 − 1) (𝜎1 + 𝜎2) + ( 𝑓𝑐 𝑓𝑡 + 1) √𝜎1 2 + 𝜎2 2 − 𝜎1𝜎2] < 1 As soon as failure happens in the tensile regime, a crack occurs perpendicular to the maximum principal stress direction. That means a crack coordinate system is set up and stored, defined by a relative angle with respect to the element coordinate system. Appropriate stress and stiffness tensor components (e.g. normal to the crack) are reduced according to SFSTR and SFSTI if IMOD = 0. The stress reduction takes place in a period of NCYCR time step cycles. For IMOD = 1.0 the stress and stiffness tensor are reduced by a damage model, please see below. A second crack orthogonal to the first crack is possible which can open and close independently from the first one, further reducing the element stiffness. To deal with crack closure, the current strain in principal stress direction is stored as initial crack strain (ICRIN = 0, default) or the initial crack strain is set to zero (ICRIN = 1). After failure, the crack strain is tracked, so that later crack closure will be detected. If that is the case, appropriate stress and stiffness tensor components (e.g. compressive) are reactivated so that e.g. under pressure a load could be carried and cause a nonzero stress perpendicular to the crack. If the critical number of failed integration points (NIPF) in one element is reached, all integration points over the element thickness fail as well. The default value of NIPF = 1 resembles the fact, that a crack in a glass plate immediately runs through the thickness. Starting with the Release of LS-DYNA version R10, a damage model for stress and stiffness softening can be activated with IMOD = 1. The corresponding evolution law for ILAW = 0 is given by 𝐷 = {⎧ {⎨ ⎩ 1 − 0 𝑓𝑜𝑟 𝜅 ≤ 𝜅0 𝜅0 (1 − 𝛼𝑡,𝑐 + 𝛼𝑡,𝑐𝑒−𝛽𝑡,𝑐 (𝜅−𝜅0)) 𝑒𝑙𝑠𝑒 i.e. tensile and compressive failure are treated in the same fashion. On the other hand, with ILAW = 1, the damage evolution for tensile failure is given by 𝐷 = {⎧ {⎨ ⎩ 0 𝑓𝑜𝑟 𝜅 ≤ 𝜅0 𝜅0 (1 − 𝛼𝑡 + 𝛼𝑡𝑒−𝛽𝑡 (𝜅−𝜅0)) 𝑒𝑙𝑠𝑒 1 − whereas damage for compressive failure evolves like that (more delayed stress reduction): 𝐷 = {⎧ {⎨ ⎩ 0 𝑓𝑜𝑟 𝜅 ≤ 𝜅0 𝜅0 (1 − 𝛼𝑐) − 𝛼𝑐𝑒−𝛽𝑐 (𝜅−𝜅0) 𝑒𝑙𝑠𝑒 1 − *MAT_GLASS VARIABLE DESCRIPTION 1 2 3 Crack flag: 0 = no crack, 1 = one crack, 2 = two cracks, -1 = failed under compression Direction of 1st principle stress as angle in radiant with respect to the element direction. The shell normal defines the positive angle direction. The 1st crack direction is perpendicular to the direction of 1st principle stress. Angle in radiant that defines the orthogonal to the 2nd crack direction (with respect to the element direction). *MAT_293 This is Material Type 293. This material models the behavior of pre-impregnated (prepreg) composite fibers during the high temperature preforming process. In addition to providing stress and strain, it also provides warp and weft yarn directions and stretch ratios after the forming process. The major applications of the model are for materials used in light weight automobile parts. Card 1 1 Variable MID Type A8 Card 2 1 2 RO F 2 3 ET F 3 4 EC F 4 Variable G124 G125 G126 GAMMAL Type F Card 3 1 F 2 F 3 F 4 Variable VM EPSILON THETA BULK Type F F F F 5 PR F 5 VF F 5 G F VARIABLE DESCRIPTION 6 7 8 G121 G122 G123 F 6 F 7 F 8 EF3 VF23 EM F 6 F 7 F 8 MID RO ET EC Material identification. A unique number or label not exceeding 8 characters must be specified. Continuum equivalent mass density. Tensile modulus along the fiber yarns, corresponding to the slope of the curve in Figure M293-2 in the Stable Modulus region from a uniaxial tension test. See Remark 5. Compression modulus along the fiber yarns, reversely calculated using bending tests when all the other material properties are determined. See Remark 5. VARIABLE DESCRIPTION PR G12i Poisson’s ratio. See Remark 5. Coefficients for the bias-extension angle change-engineering stress curve in Figure M293-3. G121 to G126 corresponds to the 6th order to 1st order factors of the loading curve. See Remark 5. GAMMAL Shear locking angle, in degrees. See Remark 5. VF EF3 Fiber volume fraction in the prepreg composite. Transverse compression modulus of the dry fiber. VF23 Transverse Poisson’s ratio of the dry fiber EM VM EPSILON THETA Young’s modulus of the cured resin. Poisson’s ratio of the cured resin Stretch ratio at the end of undulation stage during the uniaxial tension test. Example shown in Figure M293-2. See Remark 5. Initial angle offset between the fiber direction and the element direction. To reduce simulation error, when building the model, the elements should be aligned to the same direction as much as possible. BULK Bulk modulus of the prepreg material G Shear modulus of the prepreg material Remarks: 1. Fiber and Resin Properties. The dry fiber properties, EF3 and VF23, and the cure resin properties, EM and VM, are used to calculate the through thickness elastic modulus of the prepreg using the rule of mixture. These properties will not affect the in-plane deformation of the prepreg during the preforming simulation. 2. Shear Locking. In most of the preforming cases, the angle between the fiber yarns will not reach the shear locking state. This model is not designed for, and, therefore, not recommended for simulating shear locking. 3. BULK and G. BULK and G are used by the contact algorithm. Changing these parameters will not affect the final simulation result significantly (but it may affect the time step). 4. Model Description. Woven composite prepregs are characterized using a non- orthogonal coordinate system having two principal directions: one aligned with the longitudinal warp yarns and the other with the transverse weft yarns. Prior to deformation the warp and weft yarns are orthogonal. The directions and the fiber stretch ratios are determined from the deformation gradient. In Figure M293-1, the angles 𝛼 and 𝛽 refer to the relative of the rotation of the warp yarn coordinate to the local corotational 𝑥 coordinate and the angle between the warp and weft yarns, respectively [2,3,4]. The stress from material deformation is divided into two parts: (1) stress caused by the fiber stretch, 𝛔𝑓 , as shown in Figure M293-1 (a); (2) stress caused by the fiber rotation, 𝛔𝑚, as shown in Figure M293-1 (b). The total stress tensor, 𝛔, in the local corotational 𝑥 − 𝑦 coordinate system is the sum where the components are given below [3]: 𝑓 = 𝜎𝑦𝑥 𝜎𝑥𝑦 𝜎𝑥𝑦 𝑚 = 𝜎𝑦𝑥 𝑓 sin 2(𝛼 + 𝛽) #(2) 𝜎2 𝑓 = 𝜎1 𝑓 cos2(𝛼 + 𝛽) #(1) 𝑓 cos2 𝛼 + 𝜎2 𝜎𝑥𝑥 𝑓 = 𝑓 sin 2𝛼 + 𝜎1 𝑓 = 𝜎1 𝑓 sin2(𝛼 + 𝛽) #(3) 𝑓 sin2 𝛼 + 𝜎2 𝜎𝑦𝑦 𝑚 − 𝜎2 𝑚 + 𝜎2 𝜎1 𝜎1 𝑚 − 𝜎2 𝜎1 𝑚 + 𝜎2 𝜎1 𝑓 + 𝜎𝑥𝑥 sin(2𝛼 + 𝛽) #(5) 𝑚 − 𝜎2 𝜎1 𝜎𝑥𝑥 = 𝜎𝑥𝑥 𝑚 #(7) 𝑚 = 𝑚 = 𝑚 = 𝜎𝑦𝑦 𝜎𝑥𝑥 − + cos(2𝛼 + 𝛽) #(4) cos(2𝛼 + 𝛽) #(6) 𝜎𝑥𝑦 = 𝜎𝑦𝑥 = 𝜎𝑥𝑦 𝑓 + 𝜎𝑥𝑦 𝑚 #(8) 𝜎𝑦𝑦 = 𝜎𝑦𝑦 𝑓 + 𝜎𝑦𝑦 𝑚 #(9) 5. Material Property Characterization. The non-orthogonal stress components caused by yarn stretch and rotation at various deformation states will be char- acterized via a set of experiments, which are uniaxial tension, bias-extension and cantilever beam bending tests. All the tests need to be performed at the preforming temperature. See references [1] and [3] for more details. 𝑦 𝑓 𝜎2 𝑚 𝜎2 𝜎1 𝛽 𝛼 (a) 𝑚 𝜎1 (b ) Figure M293-1. Stress components caused by (a) stretch in fiber directions and (b) rotation of the fibers [3]. 400 350 300 250 200 150 100 50 ) ( Undulation region Stable Modulus region 0.00% 1.00% 2.00% 3.00% 4.00% 5.00% Stretch Ratio Figure M293-2. An example of the engineering stress as a function of stretch ratio from the uniaxial tension test [3]. The uniaxial tension test is used to obtain the fiber direction undulation strains and the stable tensile moduli, together with the in-plane Poisson’s ratio (PR). A typical test result is shown in Figure M293-2. From the stretch ratio- engineering stress curve, the tensile modulus, ET, and the stretch ratio at the end of undulation, EPSILON, can be captured. The bias-extension test is used to characterize the shear behavior of the compo- site needed for fields G12𝑖. The test procedure comes from the benchmark test literature [1]. An example of the bias-extension test angle change-engineering stress curve is shown in Figure M293-3. ) ( 0.1 0.08 0.06 0.04 0.02 Curve fitting 0.2 0.4 1.0 Angle change (radians) 0.6 0.8 1.2 1.4 Figure M293-3. An example of the angle change-engineering stress curve from the bias-extension test. The curve fit for this example is 𝑦 = −0.29𝑥6 + 1.09𝑥5 − 1.68𝑥4 + 1.37𝑥3 − 0.56𝑥2 + 0.12𝑥 . For this example curve the inputs into LS-DYNA are G121 = −0.29, G122 = 1.09, G123 = −1.68, G124 = 1.37, G125 = −0.56, and G126 = −0.12 [3]. Thermometer Forming Temp Ruler Composite Support & Clamp Heating Chamber Figure M293-4. Bending test setup [3] The angle change is calculated by using the equation [1]: 𝛾 = − 2 cos−1 𝐷 + 𝑑 √2𝐷 where 𝑑 is the cross-head displacement and 𝐷 is the difference between the original height and the original width of the sample. This equation holds only before the shear locking angle, specified in field GAMMAL, which is measured directly at the end of the test, so the curve should end when the fiber yarn angle reaches the shear locking state. The bending test should be performed to characterize the compression modulus along the yarn directions, as specified in the EC field. The test setup is shown in Figure M293-4. The composite specimen is held in a clamp and deforms under its own gravity. During the test, the composite is heated to the preform- ing temperature and the tip displacement is recorded. Due to the nonlinearity of the tensile modulus, the compression modulus is reversely calculated using a simulation: it is adjusted until the simulation leads to similar tip displacement to the real experiment case. The starting point for the compression modulus iteration can be set as about 100X of the shear modulus when the warp and weft yarns are perpendicular to each other. 6. Element Type. The material model is available for shell elements with OSU=1 and INN=2 in the CONTROL_ACCURACY card. It is recommended to use a double precision version of LS-DYNA. References: [1] J. Cao, R. Akkerman, P. Boisse, J. Chen, H.S. Cheng, E.F. de Graaf, J.L. Gorczyca, P. Harrison, G. Hivet, J. Launay, W. Lee, L. Liu, S.V. Lomov, A. Long, E. de Luycker, F. Morestin, J. Padvoiskis, X.Q. Peng, J. Sherwood, Tz. Stoilova, X.M. Tao, I. Verpoest, A. Willems, J. Wiggers, T.X. Yu, B. Zhu, Characterization of mechanical behavior of woven fabrics: Experimental methods and benchmark results, Composites Part A: Applied Science and Manufacturing, Volume 39, Issue 6, 2008, Pages 1037-1053, ISSN 1359-835X. [2] Pu Xue, Xiongqi Peng, Jian Cao, A non-orthogonal constitutive model for characterizing woven composites, Composites Part A: Applied Science and Manufacturing, Volume 34, Issue 2, 2003, Pages 183-193, ISSN 1359-835X. [3] Weizhao Zhang, Huaqing Ren, Biao Liang, Danielle Zeng, Xuming Su, Jeffrey Dahl, Mansour Mirdamadi, Qiangsheng Zhao, Jian Cao, A non-orthogonal material model of woven composites in the preforming process, CIRP Annals - Manufacturing Technology, Volume 66, Issue 1, 2017, Pages 257-260, ISSN 0007- 8506. [4] X.Q. Peng, J. Cao, A continuum mechanics-based non-orthogonal constitutive model for woven composite fabrics, Composites Part A: Applied Science and Manufacturing, Volume 36, Issue 6, 2005, Pages 859-874, ISSN 1359-835X. See *MAT_VACUUM or *MAT_140. *MAT_ALE_01 *MAT_ALE_GAS_MIXTURE This may also be referred to as *MAT_ALE_02. This model is used to simulate thermally equilibrated ideal gas mixtures. This only works with the multi-material ALE formulation (ELFORM = 11 in *SECTION_SOLID). This keyword needs to be used together with *INITIAL_GAS_MIXTURE for the initialization of gas densities and temperatures. When applied in the context of ALE airbag modeling, the injection of inflator gas is done with a *SECTION_POINT_SOURCE_MIXTURE command which controls the injection process. This is an identical material model to the *MAT_GAS_- MIXTURE model. Card 1 1 2 3 4 5 6 7 8 Variable MID IADIAB RUNIV Type A8 Default none Remark I 0 5 F 0.0 1 Card 2 for Per mass Calculation. Method (A) RUNIV = blank or 0.0. Card 2 1 2 3 4 5 6 7 8 Variable CVmass1 CVmass2 CVmass3 CVmass4 CVmass5 CVmass6 CVmass7 Cvmass8 Type F F F F F F F F Default none none none none none none none none Card 3 for Per mass Calculation. Method (A) RUNIV = blank or 0.0. Card 3 1 2 3 4 5 6 7 8 Variable CPmass1 CPmass2 CPmass3 CPmass4 CPmass5 CPmass6 CPmass7 Cpmass8 Type F F F F F F F F Default none none none none none none none none Card 2 for Per Mole Cclculation. Method (B) RUNIV is nonzero. Card 2 1 2 3 4 5 6 7 8 Variable MOLWT1 MOLWT2 MOLWT3 MOLWT4 MOLWT5 MOLWT6 MOLWT7 MOLWT8 Type F F F F F F F F Default none none none none none none none none Remark 2 Card 3 for Per Mole Cclculation. Method (B) RUNIV is nonzero. Card 3 1 2 3 4 5 6 7 8 Variable CPmole1 CPmole2 CPmole3 CPmole4 CPmole5 CPmole6 Cpmole7 CPmole8 Type F F F F F F F F Default none none none none none none none none Remark Card 4 for Per Mole Cclculation. Method (B) RUNIV is nonzero. Card 4 Variable 1 B1 Type F 2 B2 F 3 B3 F 4 B4 F 5 B5 F 6 B6 F 7 B7 F 8 B8 F Default none none none none none none none none Remark 2 Card 5 for Per Mole Cclculation. Method (B) RUNIV is nonzero. Card 5 Variable 1 C1 Type F 2 C2 F 3 C3 F 4 C4 F 5 C5 F 6 C6 F 7 C7 F 8 C8 F Default none none none none none none none none Remark 2 VARIABLE MID DESCRIPTION Material identification. A unique number or label not exceeding 8 characters must be specified. IADIAB This flag (default = 0) is used to turn ON/OFF adiabatic compression logics for an ideal gas (remark 5). EQ.0: OFF (default) EQ.1: ON RUNIV Universal gas constant in per-mole unit (8.31447 J/(mole*K)). CVmass1 - CVmass8 If RUNIV is BLANK or zero (method A): Heat capacity at constant volume for up to eight different gases in per-mass unit. VARIABLE DESCRIPTION CPmass1 - CPmass8 If RUNIV is BLANK or zero (method A): Heat capacity at constant pressure for up to eight different gases in per-mass unit. MOLWT1 - MOLWT8 If RUNIV is nonzero (method B): Molecular weight of each ideal gas in the mixture (mass-unit/mole). If RUNIV is nonzero (method B): Heat capacity at constant pressure for up to eight different gases in per-mole unit. These are nominal heat capacity values typically at STP. These are denoted by the variable “A” in the equation in remark 2. If RUNIV is nonzero (method B): First order coefficient for a temperature dependent heat capacity at constant pressure for up to eight different gases. These are denoted by the variable “B” in the equation in remark 2. If RUNIV is nonzero (method B): Second order coefficient for a temperature dependent heat capacity at constant pressure for up to eight different gases. These are denoted by the variable “C” in the equation in remark 2. CPmole1 - CPmole8 B1 - B8 C1 - C8 Remarks: 1. There are 2 methods of defining the gas properties for the mixture. If RUNIV is BLANK or ZERO → Method (A) is used to define constant heat capacities where per-mass unit values of Cv and Cp are input. Only cards 2 and 3 are required for this method. Method (B) is used to define constant or temperature dependent heat capacities where per-mole unit values of Cp are input. Cards 2- 5 are required for this method. 2. The per-mass-unit, temperature-dependent, constant-pressure heat capacity is 𝐶𝑝(𝑇) = (CPMOLE + B × 𝑇 + C × 𝑇2) MOLWT Typical metric units: 𝐶𝑝(𝑇) kg 𝐾 CPMOLE A mole K mole K2 mole K3 3. The initial temperature and the density of the gas species present in a mesh or part at time zero is specified by the keyword *INITIAL_GAS_MIXTURE. 4. The ideal gas mixture is assumed to be thermal equilibrium, that is, all species are at the same temperature (T). The gases in the mixture are also assumed to follow Dalton’s Partial Pressure Law, ngas 𝑃 = ∑ 𝑃𝑖 . The partial pressure of each gas is then 𝑃𝑖 = 𝜌𝑖𝑅gas𝑖 𝑇 Where 𝑅gas𝑖 = 𝑅univ MOLWT . The individual gas species temperature equals the mixture temperature. The temperature is computed from the internal energy where the mixture internal energy per unit volume is used, whence 𝑇 = 𝑇𝑖 = 𝑒𝑉 ngas ∑ 𝜌𝑖𝐶𝑉𝑖 ngas 𝑒𝑉 = ∑ 𝜌𝑖𝐶𝑉𝑖 ngas 𝑇𝑖 = ∑ 𝜌𝑖𝐶𝑉𝑖 𝑇. In general, the advection step conserves momentum and internal energy, but not kinetic energy. This can result in energy lost in the system and lead to a pressure drop. In *MAT_GAS_MIXTURE the dissipated kinetic energy is au- tomatically stored in the internal energy. Thus in effect the total energy is con- served instead of conserving just the internal energy. This numerical scheme has been shown to improve accuracy in some cases. However, the user should always be vigilant and check the physics of the problem closely. 5. As an example consider an airbag surrounded by ambient air. As the inflator gas flows into the bag, the ALE elements cut by the airbag fabric shell elements will contain some inflator gas inside and some ambient air outside. The multi- material element treatment is not perfect. Consequently the temperature of the outside air may, occasionally, be made artificially high after the multi-material element treatment. To prevent the outside ambient air from getting artificially high T, set IDIAB = 1 for the ambient air outside. Simple adiabatic compression equation is then assumed for the outside air. The use of this flag may be need- ed, but only when that outside air is modeled by the *MAT_GAS_MIXTURE card. Example: Consider a tank test model where the Lagrangian tank (Part S1) is surrounded by an ALE air mesh (Part H4 = AMMGID 1). There are 2 ALE parts which are defined but initially have no corresponding mesh: part 5 (H5 = AMMGID 2) is the resident gas inside the tank at t = 0, and part 6 (H6 = AMMGID 2) is the inflator gas(es) which is injected into the tank when t > 0. AMMGID stands for ALE Multi-Material Group ID. Please see figure and input below. The *MAT_GAS_MIXTURE (MGM) card defines the gas properties of ALE parts H5 & H6. The MGM card input for both method (A) and (B) are shown. The *INITIAL_GAS_MIXTURE card is also shown. It basically specifies that “AM- MGID 2 may be present in part or mesh H4 at t = 0, and the initial density of this gas is defined in the rho1 position which corresponds to the 1st material in the mixture (or H5, the resident gas).” Example configuration: Cut-off view S1 = tank H4 = AMMG1 = backgrou nd outside air (initially defined ALE mesh) H5 = AMMG2 = initial gas inside the tank (this has no initial mesh) H6 = AMMG2 = inflator gas(es) injected in (this has no initial mesh) Sample input: $------------------------------------------------------------------------------- *PART H5 = initial gas inside the tank $ PID SECID MID EOSID HGID GRAV ADPOPT TMID 5 5 5 0 5 0 0 *SECTION_SOLID 5 11 0 $------------------------------------------------------------------------------- $ Example 1: Constant heat capacities using per-mass unit. $*MAT_GAS_MIXTURE $ MID IADIAB R_univ $ 5 0 0 $ Cv1_mas Cv2_mas Cv3_mas Cv4_mas Cv5_mas Cv6_mas Cv7_mas Cv8_mas $718.7828911237.56228 $ Cp1_mas Cp2_mas Cp3_mas Cp4_mas Cp5_mas Cp6_mas Cp7_mas Cp8_mas $1007.00058 1606.1117 $------------------------------------------------------------------------------- $ Example 2: Variable heat capacities using per-mole unit. *MAT_GAS_MIXTURE $ MID IADIAB R_univ 5 0 8.314470 $ MW1 MW2 MW3 MW4 MW5 MW6 MW7 MW8 0.0288479 0.02256 $ Cp1_mol Cp2_mol Cp3_mol Cp4_mol Cp5_mol Cp6_mol Cp7_mol Cp8_mol 29.049852 36.23388 $ B1 B2 B3 B4 B5 B6 B7 B8 7.056E-3 0.132E-1 $ C1 C2 C3 C4 C5 C6 C7 C8 -1.225E-6 -0.190E-5 $------------------------------------------------------------------------------- $ One card is defined for each AMMG that will occupy some elements of a mesh set *INITIAL_GAS_MIXTURE $ SID STYPE MMGID T0 4 1 1 298.15 $ RHO1 RHO2 RHO3 RHO4 RHO5 RHO6 RHO7 RHO8 1.17913E-9 *INITIAL_GAS_MIXTURE $ SID STYPE MMGID T0 4 1 2 298.15 $ RHO1 RHO2 RHO3 RHO4 RHO5 RHO6 RHO7 RHO8 1.17913E-9 $------------------------------------------------------------------------------- F 0.0 *MAT_ALE_VISCOUS *MAT_ALE_VISCOUS *MAT_ALE_03 This may also be referred to as MAT_ALE_03. This “fluid-like” material model is very similar to Material Type 9 (*MAT_NULL). It allows the modeling of non-viscous fluids with constant or variable viscosity. The variable viscosity is a function of an equivalent deviatoric strain rate. If inviscid material is modeled, the deviatoric or viscous stresses are zero, and the equation of state supplies the pressures (or diagonal components of the stress tensor). All *MAT_ALE_cards apply only to ALE element formulation. Card 1 1 Variable MID Type I 2 RO F 3 PC F 4 5 6 7 8 MULO MUHI RK Not used RN F F F Defaults none none 0.0 0.0 0.0 0.0 VARIABLE DESCRIPTION MID Material identification. A unique number has to be chosen. RO PC Mass density. Pressure cutoff (≤ 0.0). See Remark 4. MULO There are 4 possible cases : 1. 2. 3. 4. If MULO = 0.0, then inviscid fluid is assumed. If MULO > 0.0, and MUHI = 0.0 or is not defined, then this is the traditional constant dynamic viscosity coeffi- cient 𝜇. If MULO > 0.0, and MUHI > 0.0, then MULO and MUHI are lower and upper viscosity limit values for a power- law-like variable viscosity model. If MULO is negative (for example, MULO = -1), then a user-input data load curve (with LCID = 1) defining dy- namic viscosity as a function of equivalent strain rate is used. VARIABLE DESCRIPTION MUHI There are 2 possible cases: 5. 6. in If MUHI < 0.0, then the viscosity can be defined by the file dyn21.F with a routine called user f3dm9ale_userdef1. The file is part of the general us- ermat package. the If MUHI > 0.0, then this is the upper dynamic viscosity limit (default = 0.0). This is defined only if RK and RN are defined for the variable viscosity case. Variable dynamic viscosity multiplier. See Remark 6. Variable dynamic viscosity exponent. See Remark 6. RK RN Remarks: 1. Deviatoric Viscous Stress. The null material must be used with an equation- of-state. Pressure cutoff is negative in tension. A (deviatoric) viscous stress of the form 𝜎𝑖𝑗 ′ ′ = 2𝜇𝜀̇𝑖𝑗 [ 𝑚2] ~ [ 𝑚2 𝑠] [ ] is computed for nonzero 𝜇 where 𝜀̇𝑖𝑗 namic viscosity. For example, in SI unit system, 𝜇 has a unit of [Pa × s]. ′ is the deviatoric strain rate. 𝜇 is the dy- 2. Hourglass Control Issues. The null material has no shear stiffness and hourglass control must be used with care. In some applications, the default hourglass coefficient might lead to significant energy losses. In general for fluid(s), the hourglass coefficient QM should be small (in the range 10−4 to 10−6 for the standard default IHQ choice). 3. Null Material Properties. Null material has no yield strength and behaves in a fluid-like manner. 4. Numerical Cavitation. The pressure cut-off, PC, must be defined to allow for a material to “numerically” cavitate. In other words, when a material undergoes dilatation above certain magnitude, it should no longer be able to resist this dilatation. Since dilatation stress or pressure is negative, setting PC limit to a very small negative number would allow for the material to cavitate once the pressure in the material goes below this negative value. 5. Issues with Small Values of Viscosity Exponent. If the viscosity exponent is less than 1.0, RN < 1.0, then RN − 1.0 < 0.0. In this case, at very low equivalent strain rate, the viscosity can be artificially very high. MULO is then used as the viscosity value. 6. Empirical Dynamic Viscosity. The empirical variable dynamic viscosity is typically modeled as a function of equivalent shear rate based on experimental data. For an incompressible fluid, this may be written equivalently as μ(𝛾̅̅̅̅̇ ′) = RK × 𝛾̅̅̅̅̇ ′(𝑅𝑁−1) μ(𝜀̅ ̇′) = RK × 𝜀̅ ̇′(𝑅𝑁−1) The “overbar” denotes a scalar equivalence. The “dot” denotes a time deriva- tive or rate effect. And the “prime” symbol denotes deviatoric or volume pre- serving components. The equivalent shear rate components may be related to the basic definition of (small-strain) strain rate components as follows: 𝜀̇𝑖𝑗 = ( ∂𝑢𝑖 ∂𝑥𝑗 + ∂𝑢𝑗 ∂𝑥𝑖 𝛾̇𝑖𝑗 = 2𝜀̇𝑖𝑗 ) ⇒ 𝜀̇𝑖𝑗 ′ = 𝜀̇𝑖𝑗 − 𝛿𝑖𝑗 ( 𝜀̇𝑘𝑘 ) Typically, the 2nd invariant of the deviatoric strain rate tensor is defined as: The equivalent (small-strain) deviatoric strain rate is defined as: 𝐼2𝜀̅ ̇′ = [𝜀̇𝑖𝑗 ′ 𝜀̇𝑖𝑗 ′ ] 𝜀̅′̇ ≡ 2√𝐼2𝜀′̇ = √2[𝜀̇𝑖𝑗 ′ 𝜀̇𝑖𝑗 ′ ] = √4[𝜀̇12 ′ 2 + 𝜀̇23 ′ 2 + 𝜀̇31 ′ 2] + 2[𝜀̇11 ′ 2 + 𝜀̇22 ′ 2 + 𝜀̇33 ′ 2] In non-Newtonian literatures, the equivalent shear rate is sometimes defined as 𝛾̅̅̅̅̇ ≡ √ 𝛾̇𝑖𝑗𝛾̇𝑖𝑗 = √2𝜀̇𝑖𝑗𝜀̇𝑖𝑗 = √4[𝜀̇12 2 + 𝜀̇23 2 + 𝜀̇31 2 ] + 2[𝜀̇11 2 + 𝜀̇22 2 + 𝜀̇33 2 ] It turns out that, (a) for incompressible materials (𝜀̇𝑘𝑘 = 0), and (b) the shear ′ , the equivalent shear rate is algebraical- terms are equivalent when 𝑖 ≠ 𝑗→ 𝜀̇𝑖𝑗 = 𝜀̇𝑖𝑗 ly equivalent to the equivalent (small-strain) deviatoric strain rate. ̇′ = 𝛾̅̅̅̅̇ ′ 𝜀̅ *MAT_ALE_MIXING_LENGTH This may also be referred to as *MAT_ALE_04. This viscous “fluid-like” material model is an advanced form of *MAT_ALE_VISCOUS. It allows the modeling of fluid with constant or variable viscosity and a one-parameter mixing-length turbulence model. The variable viscosity is a function of an equivalent deviatoric strain rate. The equation of state supplies the pressures for the stress tensor. All *MAT_ALE_cards apply only to ALE element formulation. Card Format Card 1 1 Variable MID Type I 2 RO F 3 PC F 4 5 6 7 8 MULO MUHI RK Not used RN F F F Defaults none 0.0 0.0 0.0 0.0 0.0 Internal Flow Card. Card 2 Variable 1 LC Type F 2 C0 F 3 C1 F 4 C2 F 5 C3 F 6 C4 F 7 C5 F F 0.0 8 C6 F Defaults 0.0 0.0 0.0 0.0 0.0 0.0 0.0 0.0 External Flow Card. Card 3 Variable 1 LC Type F 2 D0 F 3 D1 F 4 D2 F 5 E0 F 6 E1 F 7 E2 F 8 Defaults 0.0 0.0 0.0 0.0 0.0 0.0 0.0 VARIABLE DESCRIPTION MID Material identification. A unique number has to be chosen. Mass density Pressure cutoff (≤ 0.0). There are 3 possible cases: (1) If MULO > 0.0, and MUHI = 0.0 or is not defined, then this is the traditional constant dynamic viscosity coefficientμ. (2) If MULO > 0.0, and MUHI > 0.0, then MULO and MUHI are lower and upper viscosity limit values. (3) If MULO is negative (for example, MULO = -1), then a user-input data load curve (with LCID = 1) defining dynamic viscosity as a function of equivalent strain rate is used. Upper dynamic viscosity limit (default = 0.0). This is defined only if RK and RN are defined for the variable viscosity case. Variable dynamic viscosity multiplier. The viscosity is computed as μ(𝜀̇′̅̅̅̅̅̅) = 𝑟𝑘 ⋅ 𝜀̇′̅̅̅̅̅̅(𝑟𝑛−1) where the equivalent deviatoric strain rate is ̅̅̅̅̅̅ = √ 𝜀′̇ [𝜀̇11 ′ 2 + 𝜀̇22 ′ 2 + 𝜀̇33 ′ 2 + 2(𝜀̇12 ′ 2 + 𝜀̇23 ′ 2 + 𝜀̇31 ′ 2)] Variable dynamic viscosity exponent . Characteristic length, 𝑙ci, of the internal turbulent domain. Internal flow mixing length polynomial coefficients. The one- parameter turbulent mixing length is computed as 𝑙𝑐𝑖 ⎡𝐶0 + 𝐶1 (1 − ⎢ ⎣ ) + ⋯ + 𝐶6 (1 − 𝑙m = 𝑙ci 𝑙𝑐𝑖 ) ⎤ ⎥ ⎦ Characteristic length, 𝑙cx, of the external turbulent domain. External flow mixing length polynomial coefficients. If 𝑦 ≤ 𝑙cx then the mixing length is computed as 𝑙𝑚 = [𝐷0 + 𝐷1𝑦 + 𝐷2𝑦2] External flow mixing length polynomial coefficients. If 𝑦 > 𝑙cx then the mixing length is computed as 𝑙𝑚 = [𝐸0 + 𝐸1𝑦 + 𝐸2𝑦2] RO PC MULO MUHI RK RN LCI C0 - C6 LCX D0 - D2 E0 - E2 Remarks: 1. The null material must be used with an equation of-state. Pressure cutoff is negative in tension. A (deviatoric) viscous stress of the form ′ 𝜎′𝑖𝑗 = 𝜇𝜀̇𝑖𝑗 𝑚2] ≈ [ is computed for nonzero 𝜇 where 𝜀̇𝑖𝑗 namic viscosity with unit of [Pa × s]. [ ] 𝑚2 𝑠] [ ′ is the deviatoric strain rate. 𝜇 is the dy- 2. The null material has no shear stiffness and hourglass control must be used with care. In some applications, the default hourglass coefficient might lead to significant energy losses. In general for fluid(s), the hourglass coefficient QM should be small (in the range 10−4 to 10−6 for the standard default IHQ choice). 3. The Null material has no yield strength and behaves in a fluid-like manner. 4. The pressure cut-off, PC, must be defined to allow for a material to “numerical- ly” cavitate. In other words, when a material undergoes dilatation above cer- tain magnitude, it should no longer be able to resist this dilatation. Since dilatation stress or pressure is negative, setting PC limit to a very small negative number would allow for the material to cavitate once the pressure in the mate- rial goes below this negative value. 5. If the viscosity exponent is less than 1.0, at very low equivalent strain rate, the viscosity can be artificially very high. MULO is then used as the viscosity val- ue. 6. Turbulence is treated simply by considering its effects on viscosity. Total effective viscosity is the sum of the laminar and turbulent viscosities, 𝜇eff = 𝜇𝑙 + 𝜇𝑡 where 𝜇eff is the effective viscosity, and 𝜇𝑡 is the turbulent viscosi- ty. 7. The turbulent viscosity is computed based on the Prandtl’s Mixing Length Model, 𝜇𝑡 = ρ𝑙𝑚 2 |∇𝐯| *MAT_ALE_INCOMPRESSIBLE See *MAT_160. *MAT_ALE_HERSCHEL This may also be referred to as MAT_ALE_06. This is the Herschel-Buckley model. It is an enhancement to the power law viscosity model in *MAT_ALE_VISCOUS(*MAT_- ALE_03). Two additional input parameters: the yield stress threshold and critical shear strain rate can be specified to model “rigid-like” material for low strain rates. It allows the modeling of non-viscous fluids with constant or variable viscosity. The variable viscosity is a function of an equivalent deviatoric strain rate. All *MAT_- ALE_cards apply only to ALE element formulation. Card 1 1 Variable MID Type I 2 RO F 3 PC F 4 5 6 7 8 MULO MUHI RK Not used RN F F F Defaults none none 0.0 0.0 0.0 0.0 F 0.0 Card 2 1 2 3 4 5 6 7 8 Variable GDOTC TAO0 Type F F Default none none VARIABLE DESCRIPTION MID Material identification. A unique number has to be chosen. RO PC Mass density. Pressure cutoff (≤ 0.0), . VARIABLE DESCRIPTION MULO There are 4 possible cases : 1. 2. 3. 4. If MULO = 0.0, then inviscid fluid is assumed. If MULO > 0.0, and MUHI = 0.0 or is not defined, then this is the traditional constant dynamic viscosity coeffi- cient 𝜇. If MULO > 0.0, and MUHI > 0.0, then MULO and MUHI are lower and upper viscosity limit values for a power- law-like variable viscosity model. If MULO is negative (for example, MULO = -1), then a user-input data load curve (with LCID = 1) defining dy- namic viscosity as a function of equivalent strain rate is used. Upper dynamic viscosity limit (default = 0.0). This is defined only if RK and RN are defined for the variable viscosity case. 𝑘; consistency factor . 𝑛; power law index . MUHI RK RN GDOTC 𝛾̇𝑐; critical shear strain rate . TAO0 𝜏0; yield stress . Remarks: 1. The null material must be used with an equation-of-state. Pressure cutoff is negative in tension. A (deviatoric) viscous stress of the form 𝜎′𝑖𝑗 = 2𝜇𝜀′̇ 𝑚2 𝑠] [ 𝑚2] ~ [ is computed for nonzero 𝜇 where 𝜀′̇ 𝑖𝑗 is the deviatoric strain rate. 𝜇 is the dy- namic viscosity. For example, in SI unit system, 𝜇 has a unit of [Pa*s]. 𝑖𝑗 ] [ 2. The null material has no shear stiffness and hourglass control must be used with care. In some applications, the default hourglass coefficient might lead to significant energy losses. In general for fluid(s), the hourglass coefficient QM should be small (in the range 1.0E-4 to 1.0E-6 for the standard default IHQ choice). 3. Null material has no yield strength and behaves in a fluid-like manner. 4. The pressure cut-off, PC, must be defined to allow for a material to “numerical- ly” cavitate. In other words, when a material undergoes dilatation above cer- tain magnitude, it should no longer be able to resist this dilatation. Since dilatation stress or pressure is negative, setting PC limit to a very small negative number would allow for the material to cavitate once the pressure in the mate- rial goes below this negative value. 5. If the viscosity exponent is less than 1.0, 𝑅𝑁 < 1.0, then 𝑅𝑁 − 1.0 < 0.0. In this case, at very low equivalent strain rate, the viscosity can be artificially very high. MULO is then used as the viscosity value. 6. The Herschel-Buckley model employs a large viscosity to model the “rigid-like” behavior for low shear strain rates (𝛾̇ < 𝛾̇𝑐). Power law is used once the yield stress is passed. 𝜇 = 𝜇0 μ(𝛾̇) = 𝜏0 𝛾̇ + 𝑘( 𝛾̇ 𝛾̇𝑐 )𝑛−1 The shear strain rate is: 𝛾̅̅̅̅̇ ≡ √ 𝛾̇𝑖𝑗𝛾̇𝑖𝑗 = √2𝜀̇𝑖𝑗𝜀̇𝑖𝑗 = √4[𝜀̇12 2 + 𝜀̇23 2 + 𝜀̇31 2 ] + 2[𝜀̇11 2 + 𝜀̇22 2 ] 2 + 𝜀̇33 *MAT_SPH_VISCOUS This may also be referred to as MAT_SPH_01. This “fluid-like” material model is very similar to Material Type 9 (*MAT_NULL). It allows the modeling of viscous fluids with constant or variable viscosity. The variable viscosity is a function of an equivalent deviatoric strain rate. If inviscid material is modeled, the deviatoric or viscous stresses are zero, and the equation of state supplies the pressures (or diagonal components of the stress tensor). Card 1 1 Variable MID Type I 2 RO F 3 PC F 4 5 MULO MUHI F F 6 RK F 7 RC F 8 RN F Defaults none none 0.0 0.0 0.0 0.0 0.0 0.0 VARIABLE DESCRIPTION MID Material identification. A unique number has to be chosen. RO PC Mass density. Pressure cutoff (≤ 0.0). See Remark 4. MULO There are 4 possible cases : 1. 2. 3. 4. If MULO = 0.0, then inviscid fluid is assumed. If MULO > 0.0, and MUHI = 0.0 or is not defined, then this is the traditional constant dynamic viscosity coeffi- cient 𝜇. If MULO > 0.0, and MUHI > 0.0, then MULO and MUHI are lower and upper viscosity limit values for a power- law-like variable viscosity model. If MULO is negative (for example, MULO = -1), then a user-input data load curve (with LCID = 1) defining dy- namic viscosity as a function of equivalent strain rate is used. VARIABLE DESCRIPTION MUHI There are 2 possible cases: 5. 6. If MUHI < 0.0, then the viscosity can be defined by the user in the file dyn21.F with a routine called f3dm9sph_ userdefin. The file is part of the general usermat package. If MUHI > 0.0, then this is the upper dynamic viscosity limit (default = 0.0). This is defined only if RK and RN are defined for the variable viscosity case. RK RC Variable dynamic viscosity multiplier. See Remark 6. Option for Cross viscosity model: See Remark 7. RC > 0.0: Cross viscosity model will be used (overwrite all other options), values of MULO, MUHI, RK and RN will be used in the Cross viscosity model. See Re- mark 7. RC ≤ 0.0: other viscosity model (decided based on above variables) will be used. RN Variable dynamic viscosity exponent. See Remark 6. Remarks: 1. Deviatoric Viscous Stress. The null material must be used with an equation- of-state. Pressure cutoff is negative in tension. A (deviatoric) viscous stress of the form ′ ′ = 2𝜇𝜀̇𝑖𝑗 𝜎𝑖𝑗 [ 𝑚2] ~ [ 𝑚2 𝑠] [ ] is computed for nonzero 𝜇 where 𝜀̇𝑖𝑗 namic viscosity. For example, in SI unit system, 𝜇 has a unit of [Pa × s]. ′ is the deviatoric strain rate. 𝜇 is the dy- 2. Hourglass Control Issues. The null material has no shear stiffness and hourglass control must be used with care. In some applications, the default hourglass coefficient might lead to significant energy losses. In general for fluid(s), the hourglass coefficient QM should be small (in the range 10−4 to 10−6 for the standard default IHQ choice). 3. Null Material Properties. Null material has no yield strength and behaves in a fluid-like manner. 4. Numerical Cavitation. The pressure cut-off, PC, must be defined to allow for a material to “numerically” cavitate. In other words, when a material undergoes dilatation above certain magnitude, it should no longer be able to resist this dilatation. Since dilatation stress or pressure is negative, setting PC limit to a very small negative number would allow for the material to cavitate once the pressure in the material goes below this negative value. 5. Issues with Small Values of Viscosity Exponent. If the viscosity exponent is less than 1.0, RN < 1.0, then RN − 1.0 < 0.0. In this case, at very low equivalent strain rate, the viscosity can be artificially very high. MULO is then used as the viscosity value. 6. Empirical Dynamic Viscosity. The empirical variable dynamic viscosity is typically modeled as a function of equivalent shear rate based on experimental data. For an incompressible fluid, this may be written equivalently as μ(𝛾̅̅̅̅̇ ′) = RK × 𝛾̅̅̅̅̇ ′(𝑅𝑁−1) μ(𝜀̅ ̇′) = RK × 𝜀̅ ̇′(𝑅𝑁−1) The “overbar” denotes a scalar equivalence. The “dot” denotes a time deriva- tive or rate effect. And the “prime” symbol denotes deviatoric or volume pre- serving components. The equivalent shear rate components may be related to the basic definition of (small-strain) strain rate components as follows: 𝜀̇𝑖𝑗 = ( ∂𝑢𝑖 ∂𝑥𝑗 + ∂𝑢𝑗 ∂𝑥𝑖 𝛾̇𝑖𝑗 = 2𝜀̇𝑖𝑗 ) ⇒ 𝜀̇𝑖𝑗 ′ = 𝜀̇𝑖𝑗 − 𝛿𝑖𝑗 ( 𝜀̇𝑘𝑘 ) Typically, the 2nd invariant of the deviatoric strain rate tensor is defined as: The equivalent (small-strain) deviatoric strain rate is defined as: 𝐼2𝜀̅ ̇′ = [𝜀̇𝑖𝑗 ′ 𝜀̇𝑖𝑗 ′ ] 𝜀̅′̇ ≡ 2√𝐼2𝜀′̇ = √2[𝜀̇𝑖𝑗 ′ 𝜀̇𝑖𝑗 ′ ] = √4[𝜀̇12 ′ 2 + 𝜀̇23 ′ 2 + 𝜀̇31 ′ 2] + 2[𝜀̇11 ′ 2 + 𝜀̇22 ′ 2 + 𝜀̇33 ′ 2] In non-Newtonian literatures, the equivalent shear rate is sometimes defined as 𝛾̅̅̅̅̇ ≡ √ 𝛾̇𝑖𝑗𝛾̇𝑖𝑗 = √2𝜀̇𝑖𝑗𝜀̇𝑖𝑗 = √4[𝜀̇12 2 + 𝜀̇23 2 + 𝜀̇31 2 ] + 2[𝜀̇11 2 + 𝜀̇22 2 + 𝜀̇33 2 ] It turns out that, (a) for incompressible materials (𝜀̇𝑘𝑘 = 0), and (b) the shear ′ , the equivalent shear rate is algebraical- terms are equivalent when 𝑖 ≠ 𝑗→ 𝜀̇𝑖𝑗 = 𝜀̇𝑖𝑗 ly equivalent to the equivalent (small-strain) deviatoric strain rate. ̇′ = 𝛾̅̅̅̅̇ ′ 𝜀̅ 7. The Cross viscous model is one of simplest and most used model for shear- thinning behavior, i.e., the fluid’s viscosity decreases with increasing of the local shear rate 𝛾̅̅̅̅̇, thus the dynamic viscosity μ is defined as a function of 𝛾̅̅̅̅̇: μ(𝛾̅̅̅̅̇ ′) = MUHI + (MULO − MUHI)/(1.0 + RK ∗ 𝛾̅̅̅̅̇ ′)𝑅𝑁−1 Where RK and RN are two positive fitting parameters, and MULO, MUHI are the limiting values of the viscosity at low and high shear rates, respectively. RK, RN, MULO and MUHI are parameters from keyword input. *MAT_S01 This is Material Type 1 for discrete elements (*ELEMENT_DISCRETE). This provides a translational or rotational elastic spring located between two nodes. Only one degree of freedom is connected. 3 4 5 6 7 8 Card 1 1 Variable MID Type A8 2 K F VARIABLE MID DESCRIPTION Material identification. A unique number or label not exceeding 8 characters must be specified. K Elastic stiffness (force/displacement) or (moment/rotation). *MAT_DAMPER_VISCOUS This is Material Type 2 for discrete elements (*ELEMENT_DISCRETE). This material provides a linear translational or rotational damper located between two nodes. Only one degree of freedom is then connected. 3 4 5 6 7 8 Card 1 1 Variable MID 2 DC Type A8 F VARIABLE DESCRIPTION MID DC Material identification. A unique number or label not exceeding 8 characters must be specified. Damping constant ment/rotation rate). (force/displacement rate) or (mo- *MAT_S03 This is Material Type 3 for discrete elements (*ELEMENT_DISCRETE). This material provides an elastoplastic translational or rotational spring with isotropic hardening located between two nodes. Only one degree of freedom is connected. Card 1 1 Variable MID Type A8 2 K F 3 KT F 4 FY F 5 6 7 8 VARIABLE DESCRIPTION MID K KT FY Material identification. A unique number or label not exceeding 8 characters must be specified. Elastic stiffness (force/displacement) or (moment/rotation). Tangent stiffness (force/displacement) or (moment/rotation). Yield (force) or (moment). *MAT_SPRING_NONLINEAR_ELASTIC This is Material Type 4 for discrete elements (*ELEMENT_DISCRETE). This material provides a nonlinear elastic translational and rotational spring with arbitrary force versus displacement and moment versus rotation, respectively. Optionally, strain rate effects can be considered through a velocity dependent scale factor. With the spring located between two nodes, only one degree of freedom is connected. Card 1 1 2 3 4 5 6 7 8 Variable MID LCD LCR Type A8 I I VARIABLE DESCRIPTION MID LCD LCR Material identification. A unique number or label not exceeding 8 characters must be specified. Load curve ID describing force versus displacement or moment versus rotation relationship. The load curve must define the response in the negative and positive quadrants and pass through point (0,0). Optional load curve describing scale factor on force or moment as a function of relative velocity or. rotational velocity, respectively. *MAT_DAMPER_NONLINEAR_VISCOUS This is Material Type 5 for discrete elements (*ELEMENT_DISCRETE). This material provides a viscous translational damper with an arbitrary force versus velocity dependency, or a rotational damper with an arbitrary moment versus rotational velocity dependency. With the damper located between two nodes, only one degree of freedom is connected. Card 1 1 2 3 4 5 6 7 8 Variable MID LCDR Type A8 I VARIABLE DESCRIPTION MID LCDR Material identification. A unique number or label not exceeding 8 characters must be specified. identification describing force versus rate-of- Load curve displacement relationship or a moment versus rate-of-rotation relationship. The load curve must define the response in the negative and positive quadrants and pass through point (0,0). *MAT_SPRING_GENERAL_NONLINEAR This is Material Type 6 for discrete elements (*ELEMENT_DISCRETE). This material provides a general nonlinear translational or rotational spring with arbitrary loading and unloading definitions. Optionally, hardening or softening can be defined. With the spring located between two nodes, only one degree of freedom is connected. Card 1 1 2 3 4 Variable MID LCDL LCDU BETA 5 TYI 6 CYI 7 8 Type A8 I I F F F VARIABLE DESCRIPTION MID LCDL LCDU Material identification. A unique number or label not exceeding 8 characters must be specified. Load curve force/torque versus displacement/rotation relationship for loading, see Figure M26-1. identification describing identification describing Load curve force/torque versus displacement/rotation relationship for unloading, see Figure M119-1. BETA Hardening parameter, 𝛽: EQ.0.0: Tensile and compressive yield with strain softening (negative or zero slope allowed in the force versus dis- placement. load curves). TYI and CYI are not imple- mented for this option. NE.0.0: Kinematic hardening without strain softening. EQ.1.0: Isotropic hardening without strain softening. Initial yield force in tension ( > 0) Initial yield force in compression ( < 0) TYI CYI Remarks: Load curve points are in the format (displacement, force or rotation, moment). The points must be in order starting with the most negative (compressive) displacement or rotation and ending with the most positive (tensile) value. The curves need not be symmetrical. The displacement origin of the “unloading” curve is arbitrary, since it will be shifted as necessary as the element extends and contracts. On reverse yielding the “loading” curve will also be shifted along the displacement re or. rotation axis. The initial tensile and compressive Yield forces (TYI and CYI) define a range within which the element remains elastic (i.e. the “loading” curve is used for both loading and unloading). If at any time the force in the element exceeds this range, the element is deemed to have yielded, and at all subsequent times the “unloading” curve is used for unloading Figure MS6-1. General Nonlinear material for discrete elements *MAT_SPRING_MAXWELL This is Material Type 7 for discrete elements (*ELEMENT_DISCRETE). This material provides a three Parameter Maxwell Viscoelastic translational or rotational spring. Optionally, a cutoff time with a remaining constant force/moment can be defined. Card 1 1 Variable MID Type A8 2 K0 F 3 KI F 4 BETA F Default 5 TC F 1020 6 FC F 0 7 8 COPT F 0 VARIABLE DESCRIPTION MID K0 KI Material identification. A unique number or label not exceeding 8 characters must be specified. 𝐾0, short time stiffness 𝐾∞, long time stiffness BETA Decay parameter. TC FC Cut off time. After this time a constant force/moment is transmitted. Force/moment after cutoff time COPT Time implementation option: EQ.0: incremental time change, NE.0: continuous time change. Remarks: The time varying stiffness K(t) may be described in terms of the input parameters as 𝐾(𝑇) = 𝐾∞ + (𝐾0 − 𝐾∞)exp (−𝛽t) This equation was implemented by Schwer [1991] as either a continuous function of time or incrementally following the approach of Herrmann and Peterson [1968]. The continuous function of time implementation has the disadvantage of the energy absorber’s resistance decaying with increasing time even without deformation. The advantage of the incremental implementation is that an energy absorber must undergo some deformation before its resistance decays, i.e., there is no decay until impact, even in delayed impacts. The disadvantage of the incremental implementation is that very rapid decreases in resistance cannot be easily matched. *MAT_SPRING_INELASTIC This is Material Type 8 for discrete elements (*ELEMENT_DISCRETE). This material provides an inelastic tension or compression only, translational or rotational spring. Optionally, a user-specified unloading stiffness can be taken instead of the maximum loading stiffness. Card 1 1 2 Variable MID LCFD Type A8 I 3 KU F 4 CTF F 5 6 7 8 VARIABLE DESCRIPTION MID LCFD KU Material identification. A unique number or label not exceeding 8 characters must be specified. Load curve identification describing arbitrary force/torque versus displacement/rotation relationship. This curve must be defined in the positive force-displacement quadrant regardless of whether the spring acts in tension or compression. Unloading stiffness (optional). The maximum of KU and the maximum loading stiffness in the force/displacement or the moment/rotation curve is used for unloading. CTF Flag for compression/tension: EQ.-1.0: tension only, EQ.0.0: default is set to 1.0, EQ.1.0: compression only. *MAT_SPRING_TRILINEAR_DEGRADING This is Material Type 13 for discrete elements (*ELEMENT_DISCRETE). This material allows concrete shearwalls to be modeled as discrete elements under applied seismic loading. It represents cracking of the concrete, yield of the reinforcement and overall failure. Under cyclic loading, the stiffness of the spring degrades but the strength does not. Card 1 1 2 Variable MID DEFL1 Type A8 F 3 F1 F 4 DEFL2 F 5 F2 F 6 DEFL3 F 7 F3 F 8 FFLAG F VARIABLE MID DESCRIPTION Material identification. A unique number or label not exceeding 8 characters must be specified. DEFL1 Deflection at point where concrete cracking occurs. F1 Force corresponding to DEFL1 DEFL2 Deflection at point where reinforcement yields F2 Force corresponding to DEFL2 DEFL3 Deflection at complete failure F3 Force corresponding to DEFL3 FFLAG Failure flag. *MAT_SPRING_SQUAT_SHEARWALL This is Material Type 14 for discrete elements (*ELEMENT_DISCRETE). This material allows squat shear walls to be modeled using discrete elements. The behavior model captures concrete cracking, reinforcement yield, ultimate strength followed by degradation of strength finally leading to collapse. Card 1 1 2 3 4 5 6 7 8 Variable MID A14 B14 C14 D14 E14 LCID FSD Type A8 F F F F F I F VARIABLE DESCRIPTION Material identification. A unique number or label not exceeding 8 characters must be specified. Material coefficient 𝐴 Material coefficient 𝐵 Material coefficient 𝐶 Material coefficient 𝐷 Material coefficient 𝐸 Load curve ID referencing the maximum strength envelope curve Sustained strength reduction factor MID A14 B14 C14 D14 E14 LCID FSD Remarks: Material coefficients 𝐴, 𝐵, 𝐶 and 𝐷 are empirically defined constants used to define the shape of the polynomial curves which govern the cyclic behavior of the discrete element. A different polynomial relationship is used to define the loading and unloading paths allowing energy absorption through hysteresis. Coefficient E is used in the definition of the path used to “jump” from the loading path to the unloading path (or vice versa) where a full hysteresis loop is not completed. The load curve referenced is used to define the force displacement characteristics of the shear wall under monotonic loading. This curve is the basis to which the polynomials defining the cyclic behavior refer to. Finally, on the second and subsequent loading / unloading cycles, the shear wall will have reduced strength. The variable FSD is the sustained strength reduction factor. *MAT_SPRING_MUSCLE This is Material Type 15 for discrete elements (*ELEMENT_DISCRETE). This material is a Hill-type muscle model with activation. It is for use with discrete elements. The LS-DYNA implementation is due to Dr. J. A. Weiss. Card 1 1 Variable MID Type A8 2 L0 F 3 VMAX F Default 1.0 4 SV F 1.0 5 A F 6 FMAX F 7 TL F 8 TV F 1.0 1.0 Card 2 1 2 3 4 5 6 7 8 Variable FPE LMAX KSH Type F F F Default 0.0 VARIABLE MID DESCRIPTION Material identification. A unique number or label not exceeding 8 characters must be specified. L0 Initial muscle length, 𝐿0. VMAX Maximum CE shortening velocity, 𝑉max. SV Scale factor, 𝑆𝑣, for 𝑉max vs. active state. LT.0: absolute value gives load curve ID GE.0: constant value of 1.0 is used A Activation level vs. time function 𝑎(𝑡). LT.0: absolute value gives load curve ID GE.0: constant value of A is used VARIABLE DESCRIPTION FMAX Peak isometric force, 𝐹max. TL Active tension vs. length function, 𝑓TL(𝐿). LT.0: absolute value gives load curve ID GE.0: constant value of 1.0 is used TV Active tension vs. velocity function, 𝑓TV(𝑉). LT.0: absolute value gives load curve ID GE.0: constant value of 1.0 is used FPE Force vs. length function, 𝑓PE, for parallel elastic element. LT.0: absolute value gives load curve ID EQ.0: exponential function is used GT.0: constant value of 0.0 is used Relative length when 𝐹PE reaches 𝐹max. Required if 𝐹PE above. Constant, 𝐾sh, governing the exponential rise of𝐹PE. Required if 𝐹PE above. LMAX KSH Remarks: The material behavior of the muscle model is adapted from the original model proposed by Hill [1938]. Reviews of this model and extensions can be found in Winters [1990] and Zajac [1989]. The most basic Hill-type muscle model consists of a contractile element (CE) and a parallel elastic element (PE) (Figure MS15-1). An additional series elastic element (SEE) can be added to represent tendon compliance. The main assumptions of the Hill model are that the contractile element is entirely stress free and freely distensible in the resting state, and is described exactly by Hill’s equation (or some variation). When the muscle is activated, the series and parallel elements are elastic, and the whole muscle is a simple combination of identical sarcomeres in series and parallel. The main criticism of Hill’s model is that the division of forces between the parallel elements and the division of extensions between the series elements is arbitrary, and cannot be made without introducing auxiliary hypotheses. However, these criticisms apply to any discrete element model. Despite these limitations, the Hill model has become extremely useful for modeling musculoskeletal dynamics, as illustrated by its widespread use today. a(t) SEE FM FCE FPE LM vM CE FM LM PE Figure MS15-1. Discrete model for muscle contraction dynamics, based on a Hill-type representation. The total force is the sum of passive force 𝐹PE and active force 𝐹CE. The passive element (PE) represents energy storage from muscle elasticity, while the contractile element (CE) represents force generation by the muscle. The series elastic element (SEE), shown in dashed lines, is often neglected when a series tendon compliance is included. Here, 𝑎(𝑡) is the activation level, 𝐿M is the length of the muscle, and 𝑉M is the shortening velocity of the muscle. When the contractile element (CE) of the Hill model is inactive, the entire resistance to elongation is provided by the PE element and the tendon load-elongation behavior. As activation is increased, force then passes through the CE side of the parallel Hill model, providing the contractile dynamics. The original Hill model accommodated only full activation - this limitation is circumvented in the present implementation by using the modification suggested by Winters (1990). The main features of his approach were to realize that the CE force-velocity input force equals the CE tension-length output force. This yields a three-dimensional curve to describe the force-velocity-length relationship of the CE. If the force-velocity y-intercept scales with activation, then given the activation, length and velocity, the CE force can be determined. Without the SEE, the total force in the muscle FM is the sum of the force in the CE and the PE because they are in parallel: 𝐹M = 𝐹PE + 𝐹CE The relationships defining the force generated by the CE and PE as a function of 𝐿M, 𝑉M and 𝑎(𝑡) are often scaled by 𝐹max, the peak isometric force (p. 80, Winters 1990), 𝐿0, the initial length of the muscle (p. 81, Winters 1990), and 𝑉max, the maximum unloaded CE shortening velocity (p. 80, Winters 1990). From these, dimensionless length and velocity can be defined: 𝐿 = 𝐿M 𝐿0 , 𝑉 = 𝑉M 𝑉max × 𝑆𝑣[𝑎(𝑡)] Here, 𝑆𝑣 scales the maximum CE shortening velocity 𝑉max and changes with activation level 𝑎(𝑡). This has been suggested by several researchers, i.e. Winters and Stark [1985]. The activation level specifies the level of muscle stimulation as a function of time. Both have values between 0 and 1. The functions 𝑆𝑣(𝑎(𝑡)) and 𝑎(𝑡) are specified via load curves in LS-DYNA, or default values of 𝑆v = 1 and 𝑎(𝑡) = 0 are used. Note that 𝐿 is always positive and that 𝑉 is positive for lengthening and negative for shortening. The relationship between 𝐹CE, 𝑉 and 𝐿 was proposed by Bahler et al. [1967]. A three- dimensional relationship between these quantities is now considered standard for computer implementations of Hill-type muscle models [Winters 1990]. It can be written in dimensionless form as: 𝐹CE = 𝑎(𝑡) × 𝐹max × 𝑓TL(𝐿) × 𝑓TV(𝑉) Here, 𝑓TL(𝐿) and 𝑓TV(𝑉) are the tension-length and tension-velocity functions for active skeletal muscle. Thus, if current values of 𝐿M, 𝑉M, and 𝑎(𝑡) are known, then 𝐹CE can be determined (Figure MS15-1). The force in the parallel elastic element 𝐹PE is determined directly from the current length of the muscle using an exponential relationship [Winters 1990]: 𝑓PE = 𝐹PE 𝐹MAX = ⎧ { { ⎨ { { ⎩ 𝐿 ≤ 1 exp(𝐾sh) − 1 {exp [ 𝐾sh 𝐿max (𝐿 − 1)] − 1} 𝐿 > 1 Here, 𝐿max is the relative length at which the force 𝐹max occurs, and 𝐾sh is a dimensionless shape parameter controlling the rate of rise of the exponential. Alternatively, the user can define a custom 𝑓PE curve giving tabular values of normalized force versus dimensionless length as a load curve. For computation of the total force developed in the muscle 𝐹M, the functions for the tension-length 𝑓TL(𝐿) and force-velocity fTV relationships used in the Hill element must be defined. These relationships have been available for over 50 years, but have been refined to allow for behavior such as active lengthening. The active tension-length curve 𝑓TL(𝐿) describes the fact that isometric muscle force development is a function of length, with the maximum force occurring at an optimal length. According to Winters, this optimal length is typically around 𝐿 = 1.05, and the force drops off for shorter or longer lengths, approaching zero force for 𝐿 = 0.4 and 𝐿 = 1.5. Thus the curve has a bell-shape. Because of the variability in this curve between muscles, the user must specify the function 𝑓𝑇𝐿(𝐿) via a load curve, specifying pairs of points representing the normalized force (with values between 0 and 1) and normalized length 𝐿. See Figure MS15-2. Figure MS15-2. Typical normalized tension-length (TL) and tension-velocity (TV) curves for skeletal muscle. The active tension-velocity relationship 𝑓TV(𝑉) used in the muscle model is mainly due to the original work of Hill. Note that the dimensionless velocity 𝑉 is used. When 𝑉 = 0, the normalized tension is typically chosen to have a value of 1.0. When 𝑉 is greater than or equal to 0, muscle lengthening occurs. As 𝑉 increases, the function is typically designed so that the force increases from a value of 1.0 and asymptotes towards a value near 1.4 ass shown in Figure MS15-2. When 𝑉 is less than zero, muscle shortening occurs and the classic Hill equation hyperbola is used to drop the normalized tension to 0 as shown in Figure MS15-2. The user must specify the function 𝑓TV(𝑉) via a load curve, specifying pairs of points representing the normalized tension (with values between 0 and 1) and normalized velocity 𝑉 Available options include: 2D Purpose: Define a seat belt material. *MAT_B01 Card 1 1 2 3 4 5 6 7 Variable MID MPUL LLCID ULCID LMIN CSE DAMP Type A8 Default 0 F 0. I 0 I 0 F F F 0.0 0.0 0.0 0.0 8 E F Bending/Compression Parameter Card. Additional card for E.GT.0. Card 2 Variable Type 1 A F 2 I F 3 J F Default 0.0 0.0 2*I 4 AS F A 8 5 F F 6 M F 7 R F 1.0e20 1.0e20 0.05 Additional card for 2D option Card 3 1 2 3 4 5 6 7 8 Variable P1DOFF Type Default I VARIABLE DESCRIPTION MID MPUL LLCID ULCID LMIN CSE Belt material number. A unique number or label not exceeding 8 characters must be specified. Mass per unit length Curve or table ID for loading. LLCID can be either a single curve (force vs. engineering strain), or a table defining a set of strain- rate dependent loading curves. Load curve identification for unloading (force vs. engineering strain). Minimum length (for elements connected to slip rings and retractors), see notes below. Optional compressive stress elimination option which applies to shell elements only (default 0.0): EQ.0.0: eliminate compressive stresses in shell fabric EQ.1.0: do not eliminate compressive stresses. This option should not be used if retractors and slip rings are pre- sent in the model. EQ.2.0: whether or not compressive stress is eliminated is decided by LS-DYNA automatically, recommended for shell belt. DAMP Optional Rayleigh damping coefficient, which applies to shell elements only. A coefficient value of 0.10 is the default corresponding to 10% of critical damping. Sometimes smaller or larger values work better. E A I J Young’s modulus for bending/compression stiffness, when positive the optional card is invoked. See remarks. Cross sectional area for bending/compression stiffness, see remarks. Area moment of inertia for bending/compression stiffness, see remarks. Torsional constant remarks. for bending/compression stiffness, see AS Shear area for bending/compression stiffness, see remarks. VARIABLE DESCRIPTION Maximum force in compression/tension, see remarks. Maximum torque, see remarks. Rotational mass scaling factor, see remarks. Part ID offset for internally created 1D, bar-type, belt parts for 2D seatbelt of this material, i.e., the IDs of newly created 1D belt parts will be P1DOFF + 1, P1DOFF + 2, … If zero, the maximum ID of user-defined parts is used as the part ID offset. F M R P1DOFF Remarks: Each belt material defines stretch characteristics and mass properties for a set of belt elements. The user enters a load curve for loading, the points of which are (Strain, Force). Strain is defined as engineering strain, i.e. Strain = current length initial length − 1.0 Another similar curve is entered to describe the unloading behavior. Both load curves should start at the origin (0,0) and contain positive force and strain values only. The belt material is tension only with zero forces being generated whenever the strain becomes negative. The first non-zero point on the loading curve defines the initial yield point of the material. On unloading, the unloading curve is shifted along the strain axis until it crosses the loading curve at the “yield” point from which unloading commences. If the initial yield has not yet been exceeded or if the origin of the (shifted) unloading curve is at negative strain, the original loading curves will be used for both loading and unloading. If the strain is less than the strain at the origin of the unloading curve, the belt is slack and no force is generated. Otherwise, forces will then be determined by the unloading curve for unloading and reloading until the strain again exceeds yield after which the loading curves will again be used. A small amount of damping is automatically included. This reduces high frequency oscillation, but, with realistic force-strain input characteristics and loading rates, does not significantly alter the overall forces-strain performance. The damping forced opposes the relative motion of the nodes and is limited by stability: 𝐷 = 0.1 × mass × relative velocity time step size In addition, the magnitude of the damping force is limited to one-tenth of the force calculated from the force-strain relationship and is zero when the belt is slack. Damping forces are not applied to elements attached to sliprings and retractors. The user inputs a mass per unit length that is used to calculate nodal masses on initialization. A “minimum length” is also input. This controls the shortest length allowed in any element and determines when an element passes through sliprings or are absorbed into the retractors. One tenth of a typical initial element length is usually a good choice. Bending and Compression Stiffness for 1D Elements: Since these elements do not possess any bending or compression stiffness, when belts are used in an implicit analysis, dynamic analysis is mandatory. However, one dimensional belt elements can be used in implicit statics by associating them with bending/compression properties as per the first optional card. Two dimensional belt elements are not supported with this feature. To achieve bending and compression stiffness in 1D belts the belt element is overlayed with a Belytschko-Schwer beam element with circular cross section. These elements have 6 degrees of freedom including rotational degrees of freedom. The material used in this context is an elastic-ideal-plastic material where the elastic part is governed by the Young’s modulus E. Two yield values, F being the maximum compression/tension force and M being the maximum torque, are used as upper bounds for the resultants. The bending/compression forces and moments from this contribution are accumulated to the force from the seatbelt itself. Since the main purpose is to eliminate the singularities in bending and compression, it is recommend- ed to choose the bending and compression properties in the optional card carefully so as to not significantly influence the overall response. For the sake of completeness, this feature is also supported by the explicit integrator; therefore, a rotational nodal mass is needed. Each of the two nodes of an element gets a contribution from the belt that is calculated as RMASS = R × (MASS/2) × I/A, where MASS indicates the total translational mass of the belt element and R is a scaling factor input by the user. The translational mass is not modified. The bending and compression properties do not affect the stable time step. If the belts are used without sliprings, then incorporating this feature is virtually equivalent to adding Belytschko- Schwer beams on top of conventional belt elements as part of a modelling strategy. If sliprings are used, this feature is necessary to properly support the flow of material through the sliprings and swapping of belt elements across sliprings. Retractors cannot be used with this feature. *MAT_THERMAL_{OPTION} Available options include: ISOTROPIC ORTHOTROPIC ISOTROPIC_TD ORTHOTROPIC_TD DISCRETE_BEAM CWM ORTHOTROPIC_TD_LC ISOTROPIC_PHASE_CHANGE ISOTROPIC_TD_LC USER_DEFINED The *MAT_THERMAL_cards allow thermal properties to be defined in coupled structural/thermal and thermal only analyses, see *CONTROL_SOLUTION. Thermal properties must be defined for all elements in such analyses. Thermal material properties are specified by a thermal material ID number (TMID), this number is independent of the material ID number (MID) defined on all other *MAT_… property cards. In the same analysis identical TMID and MID numbers may exist. The TMID and MID numbers are related through the *PART card. *MAT_THERMAL_ISOTROPIC This is thermal material type 1. It allows isotropic thermal properties to be defined. Card 1 1 2 3 4 5 6 7 8 Variable TMID TRO TGRLC TGMULT TLAT HLAT F 3 F 4 F 5 F 6 7 8 Type A8 F Card 2 Variable 1 HC Type F 2 TC F VARIABLE TMID DESCRIPTION Thermal material identification. A unique number or label not exceeding 8 characters must be specified. TRO Thermal density: EQ.0.0: default to structural density. TGRLC Thermal generation rate curve number, see *DEFINE_CURVE: GT.0: function versus time, EQ.0: use constant multiplier value, TGMULT, LT.0: function versus temperature. TGMULT Thermal generation rate multiplier: EQ.0.0: no heat generation. Phase change temperature Latent heat Specific heat Thermal conductivity TLAT HLAT HC TC *MAT_THERMAL_ORTHOTROPIC This is thermal material type 2. It allows orthotropic thermal properties to be defined. Card 1 1 2 3 4 5 6 7 8 Variable TMID TRO TGRLC TGMULT AOPT TLAT HLAT Type A8 F F F F 5 5 A2 F 5 F 6 6 A3 F 6 F 7 8 7 8 7 8 4 K3 F 4 A1 F 4 2 K1 F 2 YP F 2 D2 F 3 K2 F 3 ZP F 3 D3 F Card 2 Variable 1 HC Type F Card 3 Variable 1 XP Type F Card 4 Variable 1 D1 Type F VARIABLE TMID DESCRIPTION Thermal material identification. A unique number or label not exceeding 8 characters must be specified. TRO Thermal density: EQ.0.0: default to structural density. *MAT_THERMAL_ORTHOTROPIC DESCRIPTION TGRLC Thermal generation rate curve number, see *DEFINE_CURVE: GT.0: function versus time, EQ.0: use constant multiplier value, TGMULT, LT.0: function versus temperature. TGMULT Thermal generation rate multiplier: EQ.0.0: no heat generation. AOPT Material axes definition: EQ.0.0: locally orthotropic with material axes by element nodes N1, N2 and N4, EQ.1.0: locally orthotropic with material axes determined by a point in space and global location of element center, EQ.2.0: globally orthotropic with material axes determined by TLAT HLAT HC K1 K2 K3 vectors. Phase change temperature Latent heat Specific heat Thermal conductivity K1 in local x-direction Thermal conductivity K2 in local y-direction Thermal conductivity K3 in local z-direction XP, YP, ZP Define coordinate of point p for AOPT = 1 A1, A2, A3 Define components of vector a for AOPT = 2 D1, D2, D3 Define components of vector v for AOPT = 2 *MAT_THERMAL_ISOTROPIC_TD This is thermal material type 3. It allows temperature dependent isotropic properties to be defined. The temperature dependency is defined by specifying a minimum of two and a maximum of eight data points. The properties must be defined for the temperature range that the material will see in the analysis. Card 1 1 2 3 4 5 6 7 8 Variable TMID TRO TGRLC TGMULT TLAT HLAT Type A8 F F F F F Card 2 Variable 1 T1 Type F Card 3 Variable 1 C1 Type F Card 4 Variable 1 K1 Type F VARIABLE TMID 2 T2 F 2 C2 F 2 K2 F 3 T3 F 3 C3 F 3 K3 F 4 T4 F 4 C4 F 4 K4 F 5 T5 F 5 C5 F 5 K5 F 6 T6 F 6 C6 F 6 K6 F 7 T7 F 7 C7 F 7 K7 F 8 T8 F 8 C8 F 8 K8 F DESCRIPTION Thermal material identification. A unique number or label not exceeding 8 characters must be specified. *MAT_THERMAL_ISOTROPIC_TD DESCRIPTION TRO Thermal density: EQ.0.0 default to structural density. TGRLC Thermal generation rate curve number, see *DEFINE_CURVE: GT.0: function versus time, EQ.0: use constant multiplier value, TGMULT, LT.0: function versus temperature. TGMULT Thermal generation rate multiplier: EQ.0.0: no heat generation. TLAT HLAT Phase change temperature Latent heat T1, …, T8 Temperatures: T1, ..., T8 C1, …, C8 Specific heat at: T1, …, T8 K1, …, K8 Thermal conductivity at: T1, …, T8 *MAT_THERMAL_ORTHOTROPIC_TD This is thermal material type 4. It allows temperature dependent orthotropic properties to be defined. The temperature dependency is defined by specifying a minimum of two and a maximum of eight data points. The properties must be defined for the temperature range that the material will see in the analysis. Card 1 1 2 3 4 5 6 7 8 Variable TMID TRO TGRLC TGMULT AOPT TLAT HLAT Type A8 F F F F F F Card 2 Variable 1 T1 Type F Card 3 Variable 1 C1 Type F Card 4 1 2 T2 F 2 C2 F 2 3 T3 F 3 C3 F 3 4 T4 F 4 C4 F 4 5 T5 F 5 C5 F 5 6 T6 F 6 C6 F 6 7 T7 F 7 C7 F 7 8 T8 F 8 C8 F 8 Variable (K1)1 (K1)2 (K1)3 (K1)4 (K1)5 (K1)6 (K1)7 (K1)8 Type F Card 5 1 F 2 F 3 F 4 F 5 F 6 F 7 F 8 Variable (K2)1 (K2)2 (K2)3 (K2)4 (K2)5 (K2)6 (K2)7 (K2)8 Type F F F F F F F Card 6 1 2 3 4 5 6 7 8 Variable (K3)1 (K3)2 (K3)3 (K3)4 (K3)5 (K3)6 (K3)7 (K3)8 Type F F F F F F F 7 F 8 7 8 4 A1 F 4 5 A2 F 5 6 A3 F 6 2 YP F 2 D2 F 3 ZP F 3 D3 F Card 7 Variable 1 XP Type F Card 8 Variable 1 D1 Type F VARIABLE TMID DESCRIPTION Thermal material identification. A unique number or label not exceeding 8 characters must be specified. TRO Thermal density: EQ.0.0: default to structural density. TGRLC Thermal generation rate curve number, see *DEFINE_CURVE: GT.0: function versus time, EQ.0: use constant multiplier value, TGMULT, LT.0: function versus temperature. TGMULT Thermal generation rate multiplier: EQ.0.0: no heat generation. VARIABLE AOPT DESCRIPTION Material axes definition: : EQ.0.0: locally orthotropic with material axes by element nodes N1, N2 and N4, EQ.1.0: locally orthotropic with material axes determined by a point in space and global location of element center, EQ.2.0: globally orthotropic with material axes determined by vectors. TLAT HLAT Phase change temperature Latent heat T1 ... T8 Temperatures: T1 ... T8 C1 ... C8 Specific heat at T1 ... T8 (K1)1 ... (K1)8 (K2)1 ... (K2)8 (K3)1 ... (K3)8 Thermal conductivity K1 in local x-direction at T1 ... T8 Thermal conductivity K2 in local y-direction at T1 ... T8 Thermal conductivity K3 in local z-direction at T1 ... T8 XP, YP, ZP Define coordinate of point p for AOPT = 1 A1, A2, A3 Define components of vector a for AOPT = 2 D1, D2, D3 Define components of vector d for AOPT = 2 *MAT_THERMAL_DISCRETE_BEAM This is thermal material type 5. It defines properties for discrete beams. It is only applicable when used with *SECTION_BEAM elform = 6. Card 1 1 2 3 4 5 6 7 8 Variable TMID TRO Type A8 F Card 2 Variable 1 HC Type F 2 TC F 3 4 5 6 7 8 VARIABLE TMID DESCRIPTION Thermal material identification. A unique number or label not exceeding 8 characters must be specified. TRO Thermal density: EQ.0.0: default to structural density. Specific heat Thermal conductance (SI units are W/K) HC = (heat transfer coefficient) × (beam cross section area) [W/K] = [W / m^2 K] * [m^2] HC TC Note: A beam cross section area is not defined on the SECTION_BEAM keyword for an elform = 6 discrete beam. A beam cross section area is needed for heat transfer calculations. Therefore, the cross section area is lumped into the value entered for HC. *MAT_THERMAL_CHEMICAL_REACTION This is thermal material type 6. The chemical species making up this material undergo chemical reactions. A maximum of 8 species and 8 chemical reactions can be defined. The thermal material properties of a finite element undergoing chemical reactions are calculated based on a mixture law consisting of those chemical species currently present in the element. The dependence of the chemical reaction rate on temperature is described by the Arrhenius equation. Time step splitting is used to couple the system of ordinary differential equations describing the chemical reaction kinetics to the system of partial differential equations describing the diffusion of heat. Card 1 1 2 3 4 5 6 7 8 Variable TMID NCHSP NCHRX ICEND CEND RBEGIN GASC Type A8 I I I R R R Chemical Species Cards. Include one card for each of the NCHSP species. These cards set species properties. The dummy index i is the species number and is equal to 1 for the first species card, 2 for the second, and so on. Card 3 1 2 3 4 5 6 7 8 Variable RHOi LCCPi LCKi N0i MWi Type R I I I I Reaction Cards. Include one card for each of the NCHSP species. Each field contains the species’s coefficient for one of the NCHRX chemical reactions. See card format 3 for explanation of the species index i. Card 4 1 2 3 4 5 6 7 8 Variable RCi1 RCi2 RCi3 RCi4 RCi5 RCi6 RCi7 RCi8 Type R R R R R R R Reaction Rate Exponent Cards. Include one card for each of the NCHSP species. Each field contains the specie’s rate exponent for one of the NCHRX chemical reactions. See card format 3 for explanation of the species index i. Card 5 1 2 3 4 5 6 7 8 Variable RXi1 RXi2 RXi3 RXi4 RXi5 RXi6 RXi7 RXi8 Type R R R R R R R R Pre-exponential Factor Card. Each field contains the natural logarithm of its corresponding reaction’s pre-exponetial factor. Card 6 Variable 1 Z1 Type R 2 Z2 R 3 Z3 R 4 Z4 R 5 Z5 R 6 Z6 R 7 Z7 R 8 Z8 R Activation Energy Card. Each field contains the activation energy value for its corresponding reaction. Card 7 Variable 1 E1 Type R 2 E2 R 3 E3 R 4 E4 R 5 E5 R 6 E6 R 7 E7 R 8 E8 R Heat of Reaction Card. Each field contains the heat of reaction value for its corresponding reaction. Card 8 Variable 1 Q1 Type R 2 Q2 R 3 Q3 R 4 Q4 R 5 Q5 R 6 Q6 R 7 Q7 R 8 Q8 R VARIABLE TMID 3-12 (MAT) DESCRIPTION Thermal material identification. A unique number or label not NCHSP Number of chemical species (maximum 8) NCHRX Number of chemical reactions (maximum 8) ICEND Species number controlling reaction termination RBEGIN Chemical reaction will start when the sum of the individual chemical reaction rates are greater than RBEGIN. GASC RHOi LCCPi LCKi N0i MWi RCij RXij Zj Ej Qj Gas constant: 1.987 cal/(g-mole K), 8314. J/(kg-mole K) Density of the ith species Load curve ID specifying specific heat vs. temperature for the ith species. Load curve ID specifying thermal conductivity vs. temperature for the ith species Initial concentration fraction of the ith species Molecular weight of the ith species. Reaction coefficient for species i in reaction j. Leave blank for undefined reactions Rate exponent for species i in reaction j. Leave blank for undefined reactions. Pre-exponential factor for reaction j. Enter the value as ln(Z). Leave blank for undefined reactions. Activation energy for reaction j. Leave blank for undefined reactions. Heat of reaction for reaction j. Leave blank for undefined reactions. Rate Model for a Single Rection: Chemical reactions are usually expressed in chemical equation notation; for example, a chemical reaction involving two reactants and two products is 𝑎A + 𝑏B → 𝑔G + ℎH, (MT6.1) where A, B, G, and H are chemical species such as NaOH or HCl, and 𝑎, 𝑏, 𝑔, and ℎ are integers called stoichiometric numbers, indicating the number of molecules involved in a single reaction. The rate of reaction is the number of individual reactions per unit time. Using a stoichiometric identity, which is just an accounting relation, the rate of reaction is proportional to the rate of change in the concentrations of the species involved in the reaction. For the chemical reaction in Equation (MT6.1), the relation between concentration and rate, 𝑟, is, 𝑟 = − d[A] d𝑡 = − d[B] d𝑡 = + d[G] d𝑡 = + d[H] d𝑡 , (MT6.2) where [X] denotes the concentration of species X, and the sign depends on whether or not the species is an input, in which case the sign is negative, or a product, in which case the sign is positive. The Model This thermal material model (T06) is built on the assumption that the reaction rate depends on the concentration of the input species according to 𝑟 = 𝑘(𝑇) ∏[X]𝑝𝑋 , where 𝑋 ranges over all species, and, for each species, the exponent, 𝑝X, is determined by empirical measurement, but may be approximated by the stoichiometric number associated with 𝑋. The proportionality constant, 𝑘, is related to the cross-section for the reaction, and it depends on temperature through the Arrhenius equation: 𝑘 = 𝑍(𝑇) exp (− 𝐸𝑖 𝑅𝑇 ), where 𝑍(𝑇) is experimentally determined , 𝐸𝑖 is the activation energy , 𝑅 is the gas constant, and 𝑇 is temperature. As an example, for the chemical reaction of Equation (MT6.1) 𝑟 = 𝑍(𝑇) exp (− 𝐸𝑖 𝑅𝑇 ) [A]𝛼[B]𝛽, where the stoichiometric numbers have been used determined exponents. instead of experimentally The rate of heat generation (exothermic) and absorption (endothermic) associated with a reaction is calculated by multiplying the heat of reaction, 𝑄𝑖 , by its rate. Rate Model for a System of Reactions: For a system of coupled chemical reactions, the change in a species’s concentration is the sum of all the contributions from each individual chemical reaction: d[X] d𝑡 = ∑(±)𝑖𝑛(𝑥)𝑖𝑟𝑖 . The index i runs over all reactions; 𝑛(𝑥)𝑖 is the stoichiometric number for species X in reaction 𝑖; and where 𝑟𝑖 is the rate of reaction 𝑖. The sign (±)𝑖 is positive for reactions that have X as a product and negative for reactions that involve X as an input. Example: For the following system of reactions A → B A + B → C 2B → C ⇒ ⇒ ⇒ 𝑟1 = 𝑘1[A] 𝑟2 = 𝑘2[A][B] 𝑟3 = 𝑘3[B]2 (MT6.3) the time evolution equations are, d[A] d𝑡 d[B] d𝑡 d[C] d𝑡 = ∑ 𝑛(𝑥)𝑖𝑟𝑖 = −𝑘1[A] − 𝑘2[A][B] = ∑ 𝑛(𝑥)𝑖𝑟𝑖 = +𝑘1[A] − 𝑘2[A][B] − 2𝑘3[B]2 (MT6.4) = ∑ 𝑛(𝑥)𝑖𝑟𝑖 = + 𝑘2[A][B] + 𝑘3[B]2. The coefficients should be identically copied from (MT6.4): Card 4 1 2 3 4 5 6 7 8 Variable RC11 RC12 RC13 RC14 RC15 RC16 RC17 RC18 Value -1 -1 0 Variable RC21 RC22 RC23 RC24 RC25 RC26 RC27 RC28 Value +1 -1 -2 Variable RC31 RC32 RC33 RC34 RC35 RC36 RC37 RC38 Value 0 1 1 The exponents are likewise picked off of (MT6.3) for next set of cards in format 5: Card 5 1 2 3 4 5 6 7 8 Variable RX11 RX12 RX13 RX14 RX15 RX16 RX17 RX18 Value +1 +1 0 Variable RX21 RX22 RX23 RX24 RX25 RX26 RX27 RX28 Value 0 +1 +2 Variable RX31 RX32 RX33 RX34 RX35 RX36 RX37 RX38 Value 0 0 0 Equivalent Units (Normalized Units): The concentrations are often scaled so that each unit of reactant yields one unit of product. Systems for which each species is assigned its own unit of concentration based on stoichiometric considerations are equivalent unit systems. Being unit-agnostic, LS-DYNA is capable of working in equivalent units. However, care must be taken so that units are treated consistently, as applying a unit scaling to the time evolution equations can be nontrivial. 1. For each reaction, the experimentally measured pre-exponential coefficients carry units that depend on the reaction itself. For instance, the pre-exponential factors 𝑍1, 𝑍2, and 𝑍3 for the reactions A → B, A + B → C, and 2B → 𝐶 respec- tively will have units of [𝑍1] = [𝑍2] = [time] [time] × × [Concentration of A] [Concentration of A] × [Concentration of B] [𝑍3] = [time] × { [Concentration of B] } . Note that each prefactor has a different dimensionality. 2. The equations in (MT6.2), which relate rate to concentration change, are logically inconsistent unless all species are measured using the same units for concentration. A species-dependent system of equivalent units would require the insertion of additional conversion factors into (MT6.2) thereby changing the form of the time-evolution equations. To avoid unit consistency issues, it is recommended that reactions be defined in the same unit system that was used to measure their empirical values. Example of Equivalent Units: The reaction of Equation (MT6.3), A → B A + B → C 2B → C changes species A into species C through an intermediate which is species B. For each unit of species C that is produced, the reaction consumes two units of species A. Since this set of chemical formulae corresponds to the curing of epoxy, which is a nearly volume-preserving process, it is customary to work in a system of equivalent units that correspond to species volume fractions. The following set of equivalent units, then, is used in the published literature: 1. Whatever the starting concentration of species A is, all units are uniformly rescaled so that [A] = 1 at time zero. Per the boxed remark above, since the constants were measured with respect to these units, this consideration does not introduce new complexity. 2. Since the process preserves volume, and since one particle of species C replaces two particles of species A (and one particle of B replace one of A), the units of concentration for species C are doubled. 𝐶̃ = 2[C] Under this transformation the rate relation for C is 𝑟 = ± d[C] d𝑡 = d𝐶̃ d𝑡 . The time evolution Equations (MT6.4) become, (note [C] has been replaced by 𝐶̃) d[A] d𝑡 = ∑ 𝑛(𝑥)𝑖𝑟𝑖 = −𝑘1[A] − 𝑘2[A][B] d[B] d𝑡 d𝐶̃ d𝑡 = ∑ 𝑛(𝑥)𝑖𝑟𝑖 = +𝑘1[A] − 𝑘2[A][B] − 2𝑘3[B]2 = ∑ 𝑛(𝑥)𝑖𝑟𝑖 = + 2𝑘2[A][B] + 2𝑘3[B]2. Whence, Therefore, since d[A] d𝑡 + d[B] d𝑡 + d𝐶̃ d𝑡 = 0. [A] + [B] + 𝐶̃ = 1 for all values of time, and since concentration values cannot become negative, it is clear that [A], [B], and 𝐶̃ are volume fractions. *MAT_T07 This is thermal material type 7. It is a thermal material with temperature dependent properties that allows for material creation triggered by temperature. The acronym CWM stands for Computational Welding Mechanics and the model is intended to be used for simulating multistage weld processes in combination with the mechanical counterpart, *MAT_CWM. Card 1 1 2 3 4 5 6 7 8 Variable TMID TRO TGRLC TGMULT HDEAD TDEAD Type A8 Card 2 1 F 2 F 3 F 4 F 5 F 6 7 8 Variable LCHC LCTC TLSTART TLEND TISTART TIEND HGHOST TGHOST Type F F F F F F F F VARIABLE TMID DESCRIPTION Thermal material identification. A unique number or label not exceeding 8 characters must be specified. TRO Thermal density: EQ.0.0: default to structural density. TGRLC Thermal generation rate curve number, see *DEFINE_CURVE: GT.0: function versus time, EQ.0: use constant multiplier value, TGMULT, LT.0: function versus temperature. TGMULT Thermal generation rate multiplier: EQ.0.0: no heat generation. HDEAD Specific heat for inactive material before birth time TDEAD Thermal conductivity for inactive material before birth time LCHC *MAT_THERMAL_CWM DESCRIPTION Load curve (or table) for specific heat as function of temperature (and maximum temperature up to current time) LCTC Load curve for thermal conductivity as function of temperature TLSTART Birth temperature of material start TLEND Birth temperature of material end TISTART Birth time start TIEND Birth time end HGHOST Specific heat for ghost (quiet) material TGHOST Thermal conductivity for ghost (quiet) material Remarks: This material is initially in a quiet state, sometimes referred to as a ghost material. In this state the material has the thermal properties defined by the quiet specific heat (HGHOST) and quiet thermal conductivity (TGHOST). These should represent the void, for example, by picking a relatively small thermal conductivity. However, the ghost specific heat must be chosen with care, since the temperature must be allowed to increase at a reasonable rate due to the heat from the weld source. When the temperature reaches the birth temperature, a history variable representing the indicator of the welding material is incremented. This variable follows 𝛾(𝑡) = min [1, max (0, 𝑇max − 𝑇𝑙 end − 𝑇𝑙 𝑇𝑙 start start )] where 𝑇max = max{𝑇(𝑠)|𝑠 < 𝑡}. The effective thermal material properties are interpolated as quiet(1 − 𝛾) 𝑐 ̃𝑝 = 𝑐𝑝(𝑇, 𝑇max)𝛾 + 𝑐𝑝 𝜇̃ = 𝜇(𝑇)𝛾 + 𝜇quiet(1 − 𝛾) where 𝑐𝑝 and 𝜇 are the specific heat and thermal conductivity, respectively. Here, the specific heat, 𝑐𝑝, is either a temperature dependent curve, or a collection of temperature dependent curves, ordered in a table according to maximum temperature 𝑇𝑚𝑎𝑥. The time parameters for creating the material provide additional formulae for the final values of the thermal properties. Before the birth time 𝑡𝑖 start of the material has been reached, the specific heat 𝑐𝑝 dead and thermal conductivity 𝜇dead are used. The default values, i.e. the values used if no user input is given, are dead = 1010𝑐𝑝(𝑇, 𝑇max) 𝑐𝑝 𝜇dead = 0 Thus, the final values of the thermal properties read 𝑐𝑝 = 𝜇 = ⎧ {{{{{{ {{{{{{ ⎨ ⎩ dead 𝑐𝑝 start 𝑡 − 𝑡𝑖 end − 𝑡𝑖 𝑡𝑖 start dead + 𝑐𝑝 end 𝑡 − 𝑡𝑖 start − 𝑡𝑖 𝑡𝑖 end 𝑐 ̃𝑝 𝑐 ̃𝑝 𝜇dead start 𝑡 − 𝑡𝑖 end − 𝑡𝑖 𝑡𝑖 start + 𝜇dead end 𝑡 − 𝑡𝑖 start − 𝑡𝑖 𝑡𝑖 end 𝜇̃ 𝜇̃ ⎧ {{{{{{ {{{{{{ ⎨ ⎩ start 𝑡 ≤ 𝑡𝑖 start < 𝑡 ≤ 𝑡𝑖 𝑡𝑖 end end < 𝑡 𝑡𝑖 start 𝑡 ≤ 𝑡𝑖 start < 𝑡 ≤ 𝑡𝑖 𝑡𝑖 end . end < 𝑡 𝑡𝑖 These parameters allow the user to control when the welding layor becomes active and thereby define a multistage welding process. Prior to the birth time, the temperature is kept more or less constant due to the large specific heat, and, thus, the material is prevented from being created *MAT_THERMAL_ORTHOTROPIC_TD_LC This is thermal material type 8. It allows temperature dependent orthotropic properties to be defined by load curves. The temperature dependency is defined by specifying a minimum of two data points. The properties must be defined for the temperature range that the material will see in the analysis. Card 1 1 2 3 4 5 6 7 8 Variable TMID TRO TGRLC TGMULT AOPT TLAT HLAT F 5 5 A2 F 5 F 6 6 A3 F 6 F 7 8 7 8 7 8 Type A8 Card 2 1 F 2 F 3 F 4 Variable LCC LCK1 LCK2 LCK3 Type I I I I 4 A1 F 4 2 YP F 2 D2 F 3 ZP F 3 D3 F Card 3 Variable 1 XP Type F Card 4 Variable 1 D1 Type F VARIABLE TMID DESCRIPTION Thermal material identification. A unique number or label not exceeding 8 characters must be specified. VARIABLE DESCRIPTION TRO Thermal density: EQ.0.0: default to structural density. TGRLC Thermal generation rate curve number, see *DEFINE_CURVE: GT.0: function versus time, EQ.0: use constant multiplier value, TGMULT, LT.0: function versus temperature. TGMULT Thermal generation rate multiplier: EQ.0.0: no heat generation. AOPT Material axes definition: : EQ.0.0: locally orthotropic with material axes by element nodes N1, N2 and N4, EQ.1.0: locally orthotropic with material axes determined by a point in space and global location of element center, EQ.2.0: globally orthotropic with material axes determined by TLAT HLAT LCC LCK1 LCK2 LCK3 vectors. Phase change temperature Latent heat Load Curve Specific Heat Load Curve Thermal Conductivity K1 in local x-direction Load Curve Thermal Conductivity K2 in local y-direction Load Curve Thermal Conductivity K3 in local z-direction XP, YP, ZP Define coordinate of point p for AOPT = 1 A1, A2, A3 Define components of vector a for AOPT = 2 D1, D2, D3 Define components of vector d for AOPT = 2 *MAT_THERMAL_ORTHOTROPIC_TD_LC See *MAT_THERMAL_ORTHOTROPIC keyword for a description of the orthotropic axis options, AOPT. *MAT_THERMAL_ISOTROPIC_PHASE_CHANGE This is thermal material type 9. It allows temperature dependent isotropic properties with phase change to be defined. The latent heat of the material is defined together with the solid and liquid temperatures. The temperature dependency is defined by specifying a minimum of two and a maximum of eight data points. The properties must be defined for the temperature range that the material will see in the analysis. Card 1 1 2 3 4 5 6 7 8 Variable TMID TRO TGRLC TGMULT Type A8 F F F Card 2 Variable 1 T1 Type F Card 3 Variable 1 C1 Type F Card 4 Variable 1 K1 Type F 2 T2 F 2 C2 F 2 K2 F 3 T3 F 3 C3 F 3 K3 F 4 T4 F 4 C4 F 4 K4 F 5 T5 F 5 C5 F 5 K5 F 6 T6 F 6 C6 F 6 K6 F 7 T7 F 7 C7 F 7 K7 F 8 T8 F 8 C8 F 8 K8 Card 5 1 2 Variable SOLT LIQT Type F F 3 LH F 4 5 6 7 8 VARIABLE TMID DESCRIPTION Thermal material identification. A unique number or label not exceeding 8 characters must be specified. TRO Thermal density: EQ.0.0: default to structural density. TGRLC Thermal generation rate curve number, see *DEFINE_CURVE: GT.0: function versus time, EQ.0: use constant multiplier value, TGMULT, LT.0: function versus temperature. TGMULT Thermal generation rate multiplier: EQ.0.0: no heat generation. T1, …, T8 Temperatures (T1, …, T8) C1, …, C8 Specific heat at T1, …, T8 K1, …, K8 Thermal conductivity at T1, …, T8 Solid temperature, TS (must be < TL) Liquid temperature, TL (must be > TS) Latent heat SOLT LIQT LH Remarks: During phase change, that is between the solid and liquid temperatures, the specific heat of the material will be enhanced to account for the latent heat as follows: 𝑐(𝑡) = 𝑚 [1 − cos2𝜋 ( 𝑇 − 𝑇𝑆 𝑇𝐿 − 𝑇𝑆 )] , 𝑇𝑆 < 𝑇 < 𝑇𝐿 where 𝑇𝐿 = liquid temperature 𝑇𝑆 = solid temperature 𝑇 = temperature 𝑚 = multiplier such that 𝜆 = ∫ 𝐶(𝑇)𝑑𝑇 𝑇𝐿 𝑇𝑆 𝜆 = latent heat 𝑐 = specific heat *MAT_THERMAL_ISOTROPIC_TD_LC This is thermal material type 10. It allows isotropic thermal properties that are temperature dependent specified by load curves to be defined. The properties must be defined for the temperature range that the material will see in the analysis. Card 1 1 2 3 4 5 6 7 8 Variable TMID TRO TGRLC TGMULT Type A8 Card 2 1 F 2 F 3 F 4 Variable HCLC TCLC Type F F 5 6 7 8 VARIABLE TMID DESCRIPTION Thermal material identification. A unique number or label not exceeding 8 characters must be specified. TRO Thermal density: EQ.0.0: default to structural density. TGRLC Thermal generation rate curve number, see *DEFINE_CURVE: GT.0: function versus time, EQ.0: use constant multiplier value, TGMULT, LT.0: function versus temperature. TGMULT Thermal generation rate multiplier: EQ.0.0: no heat generation. HCLC TCLC Load curve ID specifying specific heat vs. temperature. Load curve ID specifying thermal conductivity vs. temperature. *MAT_THERMAL_USER_DEFINED These are Thermal Material Types 11 - 15. The user can supply his own subroutines. Please consult Appendix H for more information. Card 1 1 Variable MID 2 RO 3 MT 4 5 6 7 8 LMC NVH AOPT IORTHO IHVE Type A8 F F F F F F F Orthotropic Card 1. Additional card read in when IORTHO = 1. Card 2 Variable 1 XP Type F 2 YP F 3 ZP F 4 A1 F 5 A2 F 6 A3 F 7 8 Orthotropic Card 2. Additional card read in when IORTHO = 1. Card 3 Variable 1 D1 Type F 2 D2 F 3 D3 F 4 5 6 7 8 Material Parameter Cards. Set up to 8 parameters per card. Include up to 4 cards. This input ends at the next keyword (“*”) card. Card 4 Variable 1 P1 Type F 2 P2 F 3 P3 F 4 P4 F 5 P5 F 6 P6 F 7 P7 F 8 P8 F VARIABLE MID LS-DYNA R10.0 DESCRIPTION Material identification. A unique number or label not exceeding 8 VARIABLE DESCRIPTION RO MT LMC NVH AOPT Thermal mass density. User material type (11-15 inclusive). Length of material constants array. LMC must not be greater than 32. Number of history variables. Material axes option of orthotropic materials. IORTHO = 1.0. Use if EQ.0.0: locally orthotropic with material axes by element nodes N1, N2 and N4, EQ.1.0: locally orthotropic with material axes determined by a point in space and global location of element center, EQ.2.0: globally orthotropic with material axes determined by vectors. LT.0.0: the absolute value of AOPT is a coordinate system ID number (CID on *DEFINE_COORDINATE_NODES, *DEFINE_COORDINATE_SYSTEM or *DEFINE_CO- ORDINATE_VECTOR). Available in R3 version of 971 and later. IORTHO Set to 1.0 if the material is orthotropic. IHVE XP - D3 P1 ⋮ Set to 1.0 to activate exchange of history variables between mechanical and thermal user material models. Material axes orientation of orthotropic materials. IORTHO = 1.0 Use if First material parameter. ⋮ PLMC LMCth material parameter. Remarks: 1. The IHVE = 1 option makes it possible for a thermal user material subroutine to read the history variables of a mechanical user material subroutine defined for the same part and vice versa. If the integration points for the thermal and me- chanical elements are not coincident then extrapolation/interpolation is used to calculate the value when reading history variables. 2. Option TITLE is supported 3. *INCLUDE_TRANSFORM: Transformation of units is only supported for RO field and vectors on card 2 and 3. Corporate Address Livermore Software Technology Corporation P. O. Box 712 Livermore, California 94551-0712 Support Addresses Technology Software Livermore Corporation 7374 Las Positas Road Livermore, California 94551 Tel: 925-449-2500 Fax: 925-449-2507 Email: sales@lstc.com Website: www.lstc.com Technology Software Livermore Corporation 1740 West Big Beaver Road Suite 100 Troy, Michigan 48084 Tel: 248-649-4728 Fax: 248-649-6328 Disclaimer Copyright © 1992-2017 Livermore Software Technology Corporation. All Rights Reserved. LS-DYNA®, LS-OPT® and LS-PrePost® are registered trademarks of Livermore Software Technology Corporation in the United States. All other trademarks, product names and brand names belong to their respective owners. LSTC reserves the right to modify the material contained within this manual without prior notice. The information and examples included herein are for illustrative purposes only and are not intended to be exhaustive or all-inclusive. LSTC assumes no liability or responsibility whatsoever for any direct or indirect damages or inaccuracies of any type or nature that could be deemed to have resulted from the use of this manual. Any reproduction, in whole or in part, of this manual is prohibited without the prior Patents LSTC products are protected under the following patents: US Patents: 7167816, 7286972, 7308387, 7382367, 7386425, 7386428, 7392163, 7395128, 7415400, 7428713, 7472602, 7499050, 7516053, 7533577, 7590514, 7613585, 7640146, 7657394, 7660480, 7664623, 7702490, 7702494, 7945432, 7953578, 7987143, 7996344, 8050897, 8069017, 8126684, 8150668, 8165856, 8180605, 8190408, 8200458, 8200464, 8209157, 8271237, 8296109, 8306793, 8374833, 8423327, 8467997, 8489372, 8494819, 8515714, 8521484, 8577656, 8612186, 8666719, 8744825, 8768660, 8798973, 8898042, 9020784, 9098657, 9117042, 9135377, 9286422, 9292632, 9405868, 9430594, 9507892, 9607115. Japan Patents: 5090426, 5281057, 5330300, 5373689, 5404516, 5411013, 5411057, 5431133, 5520553, 5530552, 5589198, 5601961, 5775708, 5792995, 5823170, 6043146, 6043198. Patents: China ZL200910246429.8, ZL201010171603.X, ZL201010533046.1, ZL201110140142.4, ZL201210514668.9, ZL201210475617.X, ZL201310081855.7. ZL200910207380.5, ZL201010128222.3, ZL201010174074.9, ZL201110035253.9, ZL201210039535.0, ZL201210422902.5, ZL200910165817.3, ZL201010132510.6, ZL201010287263.7, ZL201110065789.5, ZL201210286459.3, ZL201210424131.3, ZL200910221325.1, ZL201010155066.X, ZL201110037461.2, ZL201110132394.2, ZL201210275406.1, ZL201310021716.5, AES AES. Copyright © 2001, Dr Brian Gladman < brg@gladman.uk.net>, Worcester, UK. All rights reserved. LICENSE TERMS The free distribution and use of this software in both source and binary form is allowed (with or without changes) provided that: 1. distributions of this source code include the above copyright notice, this list of conditions and the following disclaimer; 2. distributions in binary form include the above copyright notice, this list of conditions and the following disclaimer in the documentation and/or other associated materials; 3. the copyright holder's name is not used to endorse products built using this software without specific written permission. DISCLAIMER This software is provided 'as is' with no explicit or implied warranties in respect of any properties, including, but not limited to, correctness and fitness for purpose. Issue Date: 21/01/2002 INTRODUCTION INTRODUCTION CHRONOLOGICAL HISTORY DYNA3D originated at the Lawrence Livermore National Laboratory [Hallquist 1976]. The early applications were primarily for the stress analysis of structures subjected to a variety of impact loading. These applications required what was then significant computer resources, and the need for a much faster version was immediately obvious. Part of the speed problem was related to the inefficient implementation of the element technology which was further aggravated by the fact that supercomputers in 1976 were much slower than today’s PC. Furthermore, the primitive sliding interface treatment could only treat logically regular interfaces that are uncommon in most finite element discretizations of complicated three-dimensional geometries; consequently, defining a suitable mesh for handling contact was often very difficult. The first version contained trusses, membranes, and a choice of solid elements. The solid elements ranged from a one-point quadrature eight-noded element with hourglass control to a twenty-noded element with eight integration points. Due to the high cost of the twenty node solid, the zero energy modes related to the reduced 8-point integration, and the high frequency content which drove the time step size down, higher order elements were all but abandoned in later versions of DYNA3D. A two-dimensional version, DYNA2D, was developed concurrently. A new version of DYNA3D was released in 1979 that was programmed to provide near optimal speed on the CRAY-1 supercomputers, contained an improved sliding interface treatment that permitted triangular segments and was an order of magnitude faster than the previous contact treatment. The 1979 version eliminated structural and higher order solid elements and some of the material models of the first version. This version also included an optional element-wise implementation of the integral difference method developed by Wilkins et al. [1974]. The 1981 version [Hallquist 1981a] evolved from the 1979 version. Nine additional material models were added to allow a much broader range of problems to be modeled including explosive-structure and soil-structure interactions. Body force loads were implemented for angular velocities and base accelerations. A link was also established from the 3D Eulerian code, JOY [Couch, et. al., 1983] for studying the structural response to impacts by penetrating projectiles. An option was provided for storing element data on disk thereby doubling the capacity of DYNA3D. The 1982 version of DYNA3D [Hallquist 1982] accepted DYNA2D [Hallquist 1980] material input directly. The new organization was such that equations of state and constitutive models of any complexity could be easily added. Complete vectorization INTRODUCTION of the material models had been nearly achieved with about a 10 percent increase in execution speed over the 1981 version. In the 1986 version of DYNA3D [Hallquist and Benson 1986], many new features were added, including beams, shells, rigid bodies, single surface contact, interface friction, discrete springs and dampers, optional hourglass treatments, optional exact volume integration, and VAX/ VMS, IBM, UNIX, COS operating systems compatibility, that greatly expanded its range of applications. DYNA3D thus became the first code to have a general single surface contact algorithm. In the 1987 version of DYNA3D [Hallquist and Benson 1987] metal forming simulations and composite analysis became a reality. This version included shell thickness changes, the Belytschko-Tsay shell element [Belytschko and Tsay, 1981], and dynamic relaxation. Also included were non-reflecting boundaries, user specified integration rules for shell and beam elements, a layered composite damage model, and single point constraints. New capabilities added in the 1988 DYNA3D [Hallquist 1988] version included a cost effective resultant beam element, a truss element, a C0 triangular shell, the BCIZ triangular shell [Bazeley et al. 1965], mixing of element formulations in calculations, composite failure modeling for solids, noniterative plane stress plasticity, contact surfaces with spot welds, tie break sliding surfaces, beam surface contact, finite stonewalls, stonewall reaction forces, energy calculations for all elements, a crushable foam constitutive model, comment cards in the input, and one-dimensional slidelines. By the end of 1988 it was obvious that a much more concentrated effort would be required in the development of this software if problems in crashworthiness were to be properly solved; therefore, Livermore Software Technology Corporation was founded to continue the development of DYNA3D as a commercial version called LS-DYNA3D which was later shortened to LS-DYNA. The 1989 release introduced many enhanced capabilities including a one-way treatment of slide surfaces with voids and friction; cross-sectional forces for structural elements; an optional user specified minimum time step size for shell elements using elastic and elastoplastic material models; nodal accelerations in the time history database; a compressible Mooney-Rivlin material model; a closed-form update shell plasticity model; a general rubber material model; unique penalty specifications for each slide surface; external work tracking; optional time step criterion for 4-node shell elements; and internal element sorting to allow full vectorization of right-hand-side force assembly. During the last ten years, considerable progress has been made as may be seen in the chronology of the developments which follows. Capabilities added in 1989-1990: • arbitrary node and element numbers, INTRODUCTION • fabric model for seat belts and airbags, • composite glass model, • vectorized type 3 contact and single surface contact, • many more I/O options, • all shell materials available for 8 node thick shell, • strain rate dependent plasticity for beams, • fully vectorized iterative plasticity, • interactive graphics on some computers, • nodal damping, • shell thickness taken into account in shell type 3 contact, • shell thinning accounted for in type 3 and type 4 contact, • soft stonewalls, • print suppression option for node and element data, • massless truss elements, rivets – based on equations of rigid body dynamics, • massless beam elements, spot welds – based on equations of rigid body dynam- ics, • expanded databases with more history variables and integration points, • force limited resultant beam, • rotational spring and dampers, local coordinate systems for discrete elements, • resultant plasticity for C0 triangular element, • energy dissipation calculations for stonewalls, • hourglass energy calculations for solid and shell elements, • viscous and Coulomb friction with arbitrary variation over surface, • distributed loads on beam elements, • Cowper and Symonds strain rate model, • segmented stonewalls, • stonewall Coulomb friction, • stonewall energy dissipation, • airbags (1990), • nodal rigid bodies, • automatic sorting of triangular shells into C0 groups, • mass scaling for quasi static analyses, INTRODUCTION • user defined subroutines, • warpage checks on shell elements, • thickness consideration in all contact types, • automatic orientation of contact segments, • sliding interface energy dissipation calculations, • nodal force and energy database for applied boundary conditions, • defined stonewall velocity with input energy calculations, Capabilities added in 1991-1992: • rigid/deformable material switching, • rigid bodies impacting rigid walls, • strain-rate effects in metallic honeycomb model 26, • shells and beams interfaces included for subsequent component analyses, • external work computed for prescribed displacement/velocity/accelerations, • linear constraint equations, • MPGS database, • MOVIE database, • Slideline interface file, • automated contact input for all input types, • automatic single surface contact without element orientation, • constraint technique for contact, • cut planes for resultant forces, • crushable cellular foams, • urethane foam model with hysteresis, • subcycling, • friction in the contact entities, • strains computed and written for the 8 node thick shells, • “good” 4 node tetrahedron solid element with nodal rotations, • 8 node solid element with nodal rotations, • 2 × 2 integration for the membrane element, • Belytschko-Schwer integrated beam, • thin-walled Belytschko-Schwer integrated beam, INTRODUCTION • improved TAURUS database control, • null material for beams to display springs and seatbelts in TAURUS, • parallel implementation on Crays and SGI computers, • coupling to rigid body codes, • seat belt capability. Capabilities added in 1993-1994: • Arbitrary Lagrangian Eulerian brick elements, • Belytschko-Wong-Chiang quadrilateral shell element, • Warping stiffness in the Belytschko-Tsay shell element, • Fast Hughes-Liu shell element, • Fully integrated thick shell element, • Discrete 3D beam element, • Generalized dampers, • Cable modeling, • Airbag reference geometry, • Multiple jet model, • Generalized joint stiffnesses, • Enhanced rigid body to rigid body contact, • Orthotropic rigid walls, • Time zero mass scaling, • Coupling with USA (Underwater Shock Analysis), • Layered spot welds with failure based on resultants or plastic strain, • Fillet welds with failure, • Butt welds with failure, • Automatic eroding contact, • Edge-to-edge contact, • Automatic mesh generation with contact entities, • Drawbead modeling, • Shells constrained inside brick elements, • NIKE3D coupling for springback, • Barlat’s anisotropic plasticity, INTRODUCTION • Superplastic forming option, • Rigid body stoppers, • Keyword input, • Adaptivity, • First MPP (Massively Parallel) version with limited capabilities. • Built in least squares fit for rubber model constitutive constants, • Large hysteresis in hyperelastic foam, • Bilhku/Dubois foam model, • Generalized rubber model, Capabilities added in 1995: • Belytschko - Leviathan Shell • Automatic switching between rigid and deformable bodies. • Accuracy on SMP machines to give identical answers on one, two or more processors. • Local coordinate systems for cross-section output can be specified. • Null material for shell elements. • Global body force loads now may be applied to a subset of materials. • User defined loading subroutine. • Improved interactive graphics. • New initial velocity options for specifying rotational velocities. • Geometry changes after dynamic relaxation can be considered for initial velocities.. • Velocities may also be specified by using material or part ID’s. • Improved speed of brick element hourglass force and energy calculations. • Pressure outflow boundary conditions have been added for the ALE options. • More user control for hourglass control constants for shell elements. • Full vectorization in constitutive models for foam, models 57 and 63. • Damage mechanics plasticity model, material 81, • General linear viscoelasticity with 6 term prony series. • Least squares fit for viscoelastic material constants. • Table definitions for strain rate effects in material type 24. INTRODUCTION • Improved treatment of free flying nodes after element failure. • Automatic projection of nodes in CONTACT_TIED to eliminate gaps in the surface. • More user control over contact defaults. • Improved interpenetration warnings printed in automatic contact. • Flag for using actual shell thickness in single surface contact logic rather than the default. • Definition by exempted part ID’s. • Airbag to Airbag venting/segmented airbags are now supported. • Airbag reference geometry speed improvements by using the reference geometry for the time step size calculation. • Isotropic airbag material may now be directly for cost efficiency. • Airbag fabric material damping is specified as the ratio of critical damping. • Ability to attach jets to the structure so the airbag, jets, and structure to move together. • PVM 5.1 Madymo coupling is available. • Meshes are generated within LS-DYNA3D for all standard contact entities. • Joint damping for translational motion. • Angular displacements, rates of displacements, damping forces, etc. in JNT- FORC file. • Link between LS-NIKE3D to LS-DYNA3D via *INITIAL_STRESS keywords. • Trim curves for metal forming springback. • Sparse equation solver for springback. • Improved mesh generation for IGES and VDA provides a mesh that can directly be used to model tooling in metal stamping analyses. • Capabilities added in 1996-1997 in Version 940: • Part/Material ID’s may be specified with 8 digits. • Rigid body motion can be prescribed in a local system fixed to the rigid body. • Nonlinear least squares fit available for the Ogden rubber model. • Least squares fit to the relaxation curves for the viscoelasticity in rubber. • Fu-Chang rate sensitive foam. • 6 term Prony series expansion for rate effects in model 57-now 73 • Viscoelastic material model 76 implemented for shell elements. • Mechanical threshold stress (MTS) plasticity model for rate effects. INTRODUCTION • Thermoelastic-plastic material model for Hughes-Liu beam element. • Ramberg-Osgood soil model • Invariant local coordinate systems for shell elements are optional. • Second order accurate stress updates. • Four noded, linear, tetrahedron element. • Co-rotational solid element for foam that can invert without stability problems. • Improved speed in rigid body to rigid body contacts. • Improved searching for the a_3, a_5 and a10 contact types. • Invariant results on shared memory parallel machines with the a_n contact types. • Thickness offsets in type 8 and 9 tie break contact algorithms. • Bucket sort frequency can be controlled by a load curve for airbag applications. • In automatic contact each part ID in the definition may have unique: ◦ Static coefficient of friction ◦ Dynamic coefficient of friction ◦ Exponential decay coefficient ◦ Viscous friction coefficient ◦ Optional contact thickness ◦ Optional thickness scale factor ◦ Local penalty scale factor • Automatic beam-to-beam, shell edge-to-beam, shell edge-to-shell edge and single surface contact algorithm. • Release criteria may be a multiple of the shell thickness in types a_3, a_5, a10, 13, and 26 contact. • Force transducers to obtain reaction forces in automatic contact definitions. Defined manually via segments, or automatically via part ID’s. • Searching depth can be defined as a function of time. • Bucket sort frequency can be defined as a function of time. • Interior contact for solid (foam) elements to prevent “negative volumes.” • Locking joint • Temperature dependent heat capacity added to Wang-Nefske inflator models. • Wang Hybrid inflator model [Wang, 1996] with jetting options and bag-to-bag venting. • Aspiration included in Wang’s hybrid model [Nusholtz, Wang, Wylie, 1996]. INTRODUCTION • Extended Wang’s hybrid inflator with a quadratic temperature variation for heat capacities [Nusholtz, 1996]. • Fabric porosity added as part of the airbag constitutive model. • Blockage of vent holes and fabric in contact with structure or itself considered in venting with leakage of gas. • Option to delay airbag liner with using the reference geometry until the reference area is reached. • Birth time for the reference geometry. • Multi-material Euler/ALE fluids, ◦ 2nd order accurate formulations. ◦ Automatic coupling to shell, brick, or beam elements ◦ Coupling using LS-DYNA contact options. ◦ Element with fluid + void and void material ◦ Element with multi-materials and pressure equilibrium • Nodal inertia tensors. • 2D plane stress, plane strain, rigid, and axisymmetric elements • 2D plane strain shell element • 2D axisymmetric shell element. • Full contact support in 2D, tied, sliding only, penalty and constraint techniques. • Most material types supported for 2D elements. • Interactive remeshing and graphics options available for 2D. • Subsystem definitions for energy and momentum output. • Boundary element method for incompressible fluid dynamics and fluid-structure interaction problems. Capabilities added during 1997-1998 in Version 950: • Adaptive refinement can be based on tooling curvature with FORMING contact. • The display of drawbeads is now possible since the drawbead data is output into the D3PLOT database. • An adaptive box option, *DEFINE_BOX_ADAPTIVE, allows control over the refinement level and location of elements to be adapted. • A root identification file, ADAPT.RID, gives the parent element ID for adapted elements. • Draw bead box option, *DEFINE_BOX_DRAWBEAD, simplifies drawbead input. INTRODUCTION • The new control option, CONTROL_IMPLICIT, activates an implicit solution scheme. • 2D Arbitrary-Lagrangian-Eulerian elements are available. • 2D automatic contact is defined by listing part ID's. • 2D r-adaptivity for plane strain and axisymmetric forging simulations is available. • 2D automatic non-interactive rezoning as in LS-DYNA2D. • 2D plane strain and axisymmetric element with 2x2 selective-reduced integration are implemented. • Implicit 2D solid and plane strain elements are available. • Implicit 2D contact is available. • The new keyword, *DELETE_CONTACT_2DAUTO, allows the deletion of 2D automatic contact definitions. • The keyword, *LOAD_BEAM is added for pressure boundary conditions on 2D elements. • A viscoplastic strain rate option is available for materials: ◦ *MAT_PLASTIC_KINEMATIC ◦ *MAT_JOHNSON_COOK ◦ *MAT_POWER_LAW_PLASTICITY ◦ *MAT_STRAIN_RATE_DEPENDENT_PLASTICITY ◦ *MAT_PIECEWISE_LINEAR_PLASTICITY ◦ *MAT_RATE_SENSITIVE_POWERLAW_PLASTICITY ◦ *MAT_ZERILLI-ARMSTRONG ◦ *MAT_PLASTICITY_WITH_DAMAGE ◦ *MAT_PLASTICITY_COMPRESSION_TENSION • Material model, *MAT_Plasticity_with_DAMAGE, has a piecewise linear damage curve given by a load curve ID. • The Arruda-Boyce hyper-viscoelastic rubber model is available, see *MAT_AR- RUDA_BOYCE. • Transverse-anisotropic-viscoelastic material for heart tissue, see *MAT_- HEART_TISSUE. • Lung hyper-viscoelastic material, see *MAT_LUNG_TISSUE. • Compression/tension plasticity model, see *MAT_Plasticity_COMPRESSION_- TENSION. • The Lund strain rate model, *MAT_STEINBERG_LUND, is added to Steinberg- Guinan plasticity model. INTRODUCTION • Rate sensitive foam model, *MAT_FU_CHANG_FOAM, has been extended to include engineering strain rates, etc. • Model, *MAT_MODIFIED_Piecewise_Linear_Plasticity, is added for modeling the failure of aluminum. • Material model, *MAT_SPECIAL_ORTHOTROPIC, added for television shadow mask problems. • Erosion strain is implemented for material type, *MAT_bamman_damage. • The equation of state, *EOS_JWLB, is available for modeling the expansion of explosive gases. • The reference geometry option is extended for foam and rubber materials and can be used for stress initialization, see *INITIAL_FOAM_REFERENCE_GEOM- ETRY. • A vehicle positioning option is available for setting the initial orientation and velocities, see *INITIAL_VEHICLE_KINEMATICS. • A boundary element method is available for incompressible fluid dynamics problems. • The thermal materials work with instantaneous coefficients of thermal expan- sion: ◦ *MAT_ELASTIC_PLASTIC_THERMAL ◦ *MAT_ORTHOTROPIC_THERMAL ◦ *MAT_TEMPERATURE_DEPENDENT_ORTHOTROPIC ◦ *MAT_ELASTIC_WITH_VISCOSITY • Airbag interaction flow rate versus pressure differences. • Contact segment search option, [bricks first optional] • A through thickness Gauss integration rule with 1-10 points is available for shell elements. Previously, 5 were available. • Shell element formulations can be changed in a full deck restart. • The tied interface which is based on constraint equations, TIED_SURFACE_TO_- SURFACE, can now fail if_FAILURE, is appended. • A general failure criteria for solid elements is independent of the material type, see *MAT_ADD_EROSION • Load curve control can be based on thinning and a flow limit diagram, see *DE- FINE_CURVE_FEEDBACK. • An option to filter the spotweld resultant forces prior to checking for failure has been added the the option, *CONSTRAINED_SPOTWELD, by appending FIL- TERED_FORCE, to the keyword. INTRODUCTION • Bulk viscosity is available for shell types 1, 2, 10, and 16. • When defining the local coordinate system for the rigid body inertia tensor a local coordinate system ID can be used. This simplifies dummy positioning. • Prescribing displacements, velocities, and accelerations is now possible for rigid body nodes. • One way flow is optional for segmented airbag interactions. • Pressure time history input for airbag type, LINEAR_FLUID, can be used. • An option is available to independently scale system damping by part ID in each of the global directions. • An option is available to independently scale global system damping in each of the global directions. • Added option to constrain global DOF along lines parallel with the global axes. The keyword is *CONSTRAINED_GLOBAL. This option is useful for adaptive remeshing. • Beam end code releases are available, see *ELEMENT_BEAM. • An initial force can be directly defined for the cable material, *MAT_CABLE_- DISCRETE_BEAM. The specification of slack is not required if this option is used. • Airbag pop pressure can be activated by accelerometers. • Termination may now be controlled by contact, via *TERMINATION_CON- TACT. • Modified shell elements types 8, 10 and the warping stiffness option in the Belytschko-Tsay shell to ensure orthogonality with rigid body motions in the event that the shell is badly warped. This is optional in the Belytschko-Tsay shell and the type 10 shell. • A one point quadrature brick element with an exact hourglass stiffness matrix has been implemented for implicit and explicit calculations. • Automatic file length determination for D3PLOT binary database is now implemented. This insures that at least a single state is contained in each D3PLOT file and eliminates the problem with the states being split between files. • The dump files, which can be very large, can be placed in another directory by specifying on the execution line. d=/home/user /test/d3dump • A print flag controls the output of data into the MATSUM and RBDOUT files by part ID's. The option, PRINT, has been added as an option to the *PART key- word. INTRODUCTION • Flag has been added to delete material data from the D3THDT file. See *DATA- BASE_EXTENT_BINARY and column 25 of the 19th control card in the struc- tured input. • After dynamic relaxation completes, a file is written giving the displaced state which can be used for stress initialization in later runs. Capabilities added during 1998-2000 in Version 960: Most new capabilities work on both the MPP and SMP versions; however, the capabilities that are implemented for the SMP version only, which were not considered critical for this release, are flagged below. These SMP unique capabilities are being extended for MPP calculations and will be available in the near future. The implicit capabilities for MPP require the development of a scalable eigenvalue solver, which is under development for a later release of LS-DYNA. • Incompressible flow solver is available. Structural coupling is not yet imple- mented. • Adaptive mesh coarsening can be done before the implicit springback calculation in metal forming applications. • Two-dimensional adaptivity can be activated in both implicit and explicit calculations. (SMP version only) • An internally generated smooth load curve for metal forming tool motion can be activated with the keyword: *DEFINE_CURVE_SMOOTH. • Torsional forces can be carried through the deformable spot welds by using the contact type: *CONTACT_SPOTWELD_WITH_TORSION (SMP version only with a high priority for the MPP version if this option proves to be stable.) • Tie break automatic contact is now available via the *CONTACT_AUTOMAT- IC_…_TIEBREAK options. This option can be used for glued panels. (SMP only) • *CONTACT_RIGID_SURFACE option is now available for modeling road surfaces (SMP version only). • Fixed rigid walls PLANAR and PLANAR_FINITE are represented in the binary output file by a single shell element. • Interference fits can be modeled with the INTERFERENCE option in contact. • A layered shell theory is implemented for several constitutive models including the composite models to more accurately represent the shear stiffness of laminat- ed shells. • Damage mechanics is available to smooth the post-failure reduction of the resultant forces in the constitutive model *MAT_SPOTWELD_DAMAGE. INTRODUCTION • Finite elastic strain isotropic plasticity model is available for solid elements. *MAT_FINITE_ELASTIC_STRAIN_PLASTICITY. • A shape memory alloy material is available: *MAT_SHAPE_MEMORY. • Reference geometry for material, *MAT_MODIFIED_HONEYCOMB, can be set at arbitrary relative volumes or when the time step size reaches a limiting value. This option is now available for all element types including the fully integrated solid element. • Non orthogonal material axes are available in the airbag fabric model. See *MAT_FABRIC. • Other new constitutive models include for the beam elements: ◦ *MAT_MODIFIED_FORCE_LIMITED ◦ *MAT_SEISMIC_BEAM ◦ *MAT_CONCRETE_BEAM • for shell and solid elements: ◦ *MAT_ELASTIC_VISCOPLASTIC_THERMAL • for the shell elements: ◦ *MAT_GURSON ◦ *MAT_GEPLASTIC_SRATE2000 ◦ *MAT_ELASTIC_VISCOPLASTIC_THERMAL ◦ *MAT_COMPOSITE_LAYUP ◦ *MAT_COMPOSITE_LAYUP ◦ *MAT_COMPOSITE_DIRECT • for the solid elements: ◦ *MAT_JOHNSON_HOLMQUIST_CERAMICS ◦ *MAT_JOHNSON_HOLMQUIST_CONCRETE ◦ *MAT_INV_HYPERBOLIC_SIN ◦ *MAT_UNIFIED_CREEP ◦ *MAT_SOIL_BRICK ◦ *MAT_DRUCKER_PRAGER ◦ *MAT_RC_SHEAR_WALL • and for all element options a very fast and efficient version of the Johnson-Cook plasticity model is available: • *MAT_SIMPLIFIED_JOHNSON_COOK • A fully integrated version of the type 16 shell element is available for the resultant constitutive models. INTRODUCTION • A nonlocal failure theory is implemented for predicting failure in metallic materials. The keyword *MAT_NONLOCAL activates this option for a subset of elastoplastic constitutive models. • A discrete Kirchhoff triangular shell element (DKT) for explicit analysis with three in plane integration points is flagged as a type 17 shell element. This element has much better bending behavior than the C0 triangular element. • A discrete Kirchhoff linear triangular and quadrilateral shell element is available as a type 18 shell. This shell is for extracting normal modes and static analysis. • A C0 linear 4-node quadrilateral shell element is implemented as element type 20 with drilling stiffness for normal modes and static analysis. • An assumed strain linear brick element is available for normal modes and statics. • The fully integrated thick shell element has been extended for use in implicit calculations. • A fully integrated thick shell element based on an assumed strain formulation is now available. This element uses a full 3D constitutive model which includes the normal stress component and, therefore, does not use the plane stress assump- tion. • The 4-node constant strain tetrahedron element has been extended for use in implicit calculations. • Relative damping between parts is available, see *DAMPING_RELATIVE (SMP only). • Preload forces are can be input for the discrete beam elements. • Objective stress updates are implemented for the fully integrated brick shell element. • Acceleration time histories can be prescribed for rigid bodies. • Prescribed motion for nodal rigid bodies is now possible. • Generalized set definitions, i.e., SET_SHELL_GENERAL etc. provide much flexibility in the set definitions. • The command “sw4.” will write a state into the dynamic relaxation file, D3DRLF, during the dynamic relaxation phase if the D3DRLF file is requested in the input. • Added mass by PART ID is written into the MATSUM file when mass scaling is used to maintain the time step size, (SMP version only). • Upon termination due to a large mass increase during a mass scaled calculation a print summary of 20 nodes with the maximum added mass is printed. • Eigenvalue analysis of models containing rigid bodies is now available using BCSLIB-EXT solvers from Boeing. (SMP version only). INTRODUCTION • Second order stress updates can be activated by part ID instead of globally on the *CONTROL_ACCURACY input. • Interface frictional energy is optionally computed for heat generation and is output into the interface force file (SMP version only). • The interface force binary database now includes the distance from the contact surface for the FORMING contact options. This distance is given after the nodes are detected as possible contact candidates. (SMP version only). • Type 14 acoustic brick element is implemented. This element is a fully integrat- ed version of type 8, the acoustic element (SMP version only). • A flooded surface option for acoustic applications is available (SMP version only). • Attachment nodes can be defined for rigid bodies. This option is useful for NVH applications. • CONSTRAINED_POINTS tie any two points together. These points must lie on a shell elements. • Soft constraint is available for edge to edge contact in type 26 contact. • CONSTAINED_INTERPOLATION option for beam to solid interfaces and for spreading the mass and loads. (SMP version only). • A database option has been added that allows the output of added mass for shell elements instead of the time step size. • A new contact option allows the inclusion of all internal shell edges in contact type *CONTACT_GENERAL, type 26. This option is activated by adding “_IN- TERIOR” after the GENERAL keyword. • A new option allows the use deviatoric strain rates rather than total rates in material model 24 for the Cowper-Symonds rate model. • The CADFEM option for ASCII databases is now the default. Their option includes more significant figures in the output files. • When using deformable spot welds, the added mass for spot welds is now printed for the case where global mass scaling is activated. This output is in the log file, d3hsp file, and the messag file. • Initial penetration warnings for edge-to-edge contact are now written into the MESSAG file and the d3hsp file. • Each compilation of LS-DYNA is given a unique version number. • Finite length discrete beams with various local axes options are now available for material types 66, 67, 68, 93, and 95. In this implementation the absolute value of SCOOR must be set to 2 or 3 in the *SECTION_BEAM input. • New discrete element constitutive models are available: INTRODUCTION ◦ *MAT_ELASTIC_SPRING_DISCRETE_BEAM ◦ *MAT_INELASTIC_SPRING_DISCRETE_BEAM ◦ *MAT_ELASTIC_6DOF_SPRING_DISCRETE_BEAM ◦ *MAT_INELASTIC_6DOF_SPRING_DISCRETE_BEAM • The latter two can be used as finite length beams with local coordinate systems. • Moving SPC's are optional in that the constraints are applied in a local system that rotates with the 3 defining nodes. • A moving local coordinate system, CID, can be used to determine orientation of discrete beam elements. • Modal superposition analysis can be performed after an eigenvalue analysis. Stress recovery is based on type 18 shell and brick (SMP only). • Rayleigh damping input factor is now input as a fraction of critical damping, i.e. 0.10. The old method required the frequency of interest and could be highly unstable for large input values. • Airbag option “SIMPLE_PRESSURE_VOLUME” allows for the constant CN to be replaced by a load curve for initialization. Also, another load curve can be defined which allows CN to vary as a function of time during dynamic relaxa- tion. After dynamic relaxation CN can be used as a fixed constant or load curve. • Hybrid inflator model utilizing CHEMKIN and NIST databases is now available. Up to ten gases can be mixed. • Option to track initial penetrations has been added in the automatic SMP contact types rather than moving the nodes back to the surface. This option has been available in the MPP contact for some time. This input can be defined on the fourth card of the *CONTROL_CONTACT input and on each contact definition on the third optional card in the *CONTACT definitions. • If the average acceleration flag is active, the average acceleration for rigid body nodes is now written into the D3THDT and NODOUT files. In previous versions of LS-DYNA, the accelerations on rigid nodes were not averaged. • A capability to initialize the thickness and plastic strain in the crash model is available through the option *INCLUDE_STAMPED_PART, which takes the results from the LS-DYNA stamping simulation and maps the thickness and strain distribution onto the same part with a different mesh pattern. • A capability to include finite element data from other models is available through the option, *INCLUDE_TRANSFORM. This option will take the model defined in an INCLUDE file: offset all ID's; translate, rotate, and scale the coordi- nates; and transform the constitutive constants to another set of units. INTRODUCTION Features added during 2001-2002 for the 970 release of LS-DYNA: Some of the new features, which are also listed below, were also added to later releases of version 960. Most new explicit capabilities work for both the MPP and SMP versions; however, the implicit capabilities for MPP require the development of a scalable eigenvalue solver and a parallel implementation of the constraint equations into the global matrices. This work is underway. A later release of version 970 is planned in 2003 that will be scalable for implicit solutions. Below is list of new capabilities and features: • MPP decomposition can be controlled using *CONTROL_MPP_DECOMPOSI- TION commands in the input deck. • The MPP arbitrary Lagrangian-Eulerian fluid capability now works for airbag deployment in both SMP and MPP calculations. • Euler-to-Euler coupling is now available through the keyword *CON- STRAINED_EULER_TO_EULER. • Up to ten ALE multi-material groups may now be defined. The previous limit was three groups. • Volume fractions can be automatically assigned during initialization of multi- material cells. See the GEOMETRY option of *INITIAL_VOLUME_FRACTION. • A new ALE smoothing option is available to accurately predict shock fronts. • DATABASE_FSI activates output of fluid-structure interaction data to ASCII file DBFSI. • Point sources for airbag inflators are available. The origin and mass flow vector of these inflators are permitted to vary with time. • A majority of the material models for solid materials are available for calcula- tions using the SPH (Smooth Particle Hydrodynamics) option. • The Element Free Galerkin method (EFG or meshfree) is available for two- dimensional and three-dimensional solids. This new capability is not yet im- plemented for MPP applications. • A binary option for the ASCII files is now available. This option applies to all ASCII files and results in one binary file that contains all the information normal- ly spread between a large number of separate ASCII files. • Material models can now be defined by numbers rather than long names in the keyword input. For example the keyword *MAT_PIECEWISE_LINEAR_PLAS- TICITY can be replaced by the keyword: *MAT_024. • An embedded NASTRAN reader for direct reading of NASTRAN input files is available. This option allows a typical input file for NASTRAN to be read direct- ly and used without additional input. See the *INCLUDE_NASTRAN keyword. INTRODUCTION • Names in the keyword input can represent numbers if the *PARAMETER option is used to relate the names and the corresponding numbers. • Model documentation for the major ASCII output files is now optional. This option allows descriptors to be included within the ASCII files that document the contents of the file. • ID’s have been added to the following keywords: ◦ *BOUNDARY_PRESCRIBED_MOTION ◦ *BOUNDARY_PRESCRIBED_SPC ◦ *CONSTRAINED_GENERALIZED_WELD ◦ *CONSTRAINED_JOINT ◦ *CONSTRAINED_NODE_SET ◦ *CONSTRAINED_RIVET ◦ *CONSTRAINED_SPOTWELD ◦ *DATABASE_CROSS_SECTION ◦ *ELEMENT_MASS • Penetration warnings for the contact option, ignore initial penetration, î are added as an option. Previously, no penetration warnings were written when this contact option was activated. • Penetration warnings for nodes in-plane with shell mid-surface are printed for the AUTOMATIC contact options. Previously, these nodes were ignored since it was assumed that they belonged to a tied interface where an offset was not used; consequently, they should not be treated in contact. • For the arbitrary spot weld option, the spot welded nodes and their contact segments are optionally written into the d3hsp file. See *CONTROL_CON- TACT. • For the arbitrary spot weld option, if a segment cannot be found for the spot welded node, an option now exists to error terminate. See *CONTROL_CON- TACT. • Spot weld resultant forces are written into the SWFORC file for solid elements used as spot welds. • Solid materials have now been added to the failed element report. • A new option for terminating a calculation is available, *TERMINATION_- CURVE. • A 10-noded tetrahedron solid element is available with either a 4 or 5 point integration rule. This element can also be used for implicit solutions. • A new 4 node linear shell element is available that is based on Wilson’s plate element combined with a Pian-Sumihara membrane element. This is shell type 21. INTRODUCTION • A shear panel element has been added for linear applications. This is shell type 22. This element can also be used for implicit solutions. • A null beam element for visualization is available. The keyword to define this null beam is *ELEMENT_PLOTEL. This element is necessary for compatibility with NASTRAN. • A scalar node can be defined for spring-mass systems. The keyword to define this node is *NODE_SCALAR. This node can have from 1 to 6 scalar degrees-of- freedom. • A thermal shell has been added for through-thickness heat conduction. Internally, 8 additional nodes are created, four above and four below the mid- surface of the shell element. A quadratic temperature field is modeled through the shell thickness. Internally, the thermal shell is a 12 node solid element. • A beam OFFSET option is available for the *ELEMENT_BEAM definition to permit the beam to be offset from its defining nodal points. This has the ad- vantage that all beam formulations can now be used as shell stiffeners. • A beam ORIENTATION option for orienting the beams by a vector instead of the third node is available in the *ELEMENT_BEAM definition for NASTRAN compatibility. • Non-structural mass has been added to beam elements for modeling trim mass and for NASTRAN compatibility. • An optional checking of shell elements to avoid abnormal terminations is available. See *CONTROL_SHELL. If this option is active, every shell is checked each time step to see if the distortion is so large that the element will invert, which will result in an abnormal termination. If a bad shell is detected, either the shell will be deleted or the calculation will terminate. The latter is controlled by the input. • An offset option is added to the inertia definition. See *ELEMENT_INERTIA_- OFFSET keyword. This allows the inertia tensor to be offset from the nodal point. • Plastic strain and thickness initialization is added to the draw bead contact option. See *CONTACT_DRAWBEAD_INITIALIZE. • Tied contact with offsets based on both constraint equations and beam elements for solid elements and shell elements that have 3 and 6 degrees-of-freedom per node, respectively. See BEAM_OFFSET and CONSTRAINED_OFFSET contact options. These options will not cause problems for rigid body motions. • The segment-based (SOFT = 2) contact is implemented for MPP calculations. This enables airbags to be easily deployed on the MPP version. • Improvements are made to segment-based contact for edge-to-edge and sliding conditions, and for contact conditions involving warped segments. INTRODUCTION • An improved interior contact has been implemented to handle large shear deformations in the solid elements. A special interior contact algorithm is avail- able for tetrahedron elements. • Coupling with MADYMO 6.0 uses an extended coupling that allows users to link most MADYMO geometric entities with LS-DYNA FEM simulations. In this coupling MADYMO contact algorithms are used to calculate interface forces between the two models. • Release flags for degrees-of-freedom for nodal points within nodal rigid bodies are available. This makes the nodal rigid body option nearly compatible with the RBE2 option in NASTRAN. • Fast updates of rigid bodies for metalforming applications can now be accom- plished by ignoring the rotational degrees-of-freedom in the rigid bodies that are typically inactive during sheet metal stamping simulations. See the keyword: *CONTROL_RIGID. • Center of mass constraints can be imposed on nodal rigid bodies with the SPC option in either a local or a global coordinate system. • Joint failure based on resultant forces and moments can now be used to simulate the failure of joints. • CONSTRAINED_JOINT_STIFFNESS now has a TRANSLATIONAL option for the translational and cylindrical joints. • Joint friction has been added using table look-up so that the frictional moment can now be a function of the resultant translational force. • The nodal constraint options *CONSTRAINED_INTERPOLATION and *CON- STRAINED_LINEAR now have a local option to allow these constraints to be applied in a local coordinate system. • Mesh coarsening can now be applied to automotive crash models at the beginning of an analysis to reduce computation times. See the new keyword: *CONTROL_COARSEN. • Force versus time seatbelt pretensioner option has been added. • Both static and dynamic coefficients of friction are available for seat belt slip rings. Previously, only one friction constant could be defined. • *MAT_SPOTWELD now includes a new failure model with rate effects as well as additional failure options. • Constitutive models added for the discrete beam elements: ◦ *MAT_1DOF_GENERALIZED_SPRING ◦ *MAT_GENERAL_NONLINEAR_6dof_DISCRETE_BEAM ◦ *MAT_GENERAL_NONLINEAR_1dof_DISCRETE_BEAM ◦ *MAT_GENERAL_SPRING_DISCRETE_BEAM INTRODUCTION ◦ *MAT_GENERAL_JOINT_DISCRETE_BEAM ◦ *MAT_SEISMIC_ISOLATOR • for shell and solid elements: ◦ *MAT_plasticity_with_damage_ortho ◦ *MAT_simplified_johnson_cook_orthotropic_damage ◦ *MAT_HILL_3R ◦ *MAT_GURSON_RCDC • for the solid elements: ◦ *MAT_SPOTWELD ◦ *MAT_HILL_FOAM ◦ *MAT_WOOD ◦ *MAT_VISCOELASTIC_HILL_FOAM ◦ *MAT_LOW_DENSITY_SYNTHETIC_FOAM ◦ *MAT_RATE_SENSITIVE_POLYMER ◦ *MAT_QUASILINEAR VISCOELASTIC ◦ *MAT_TRANSVERSELY_ANISOTROPIC_CRUSHABLE_FOAM ◦ *MAT_VACUUM ◦ *MAT_MODIFIED_CRUSHABLE_FOAM ◦ *MAT_PITZER_CRUSHABLE FOAM ◦ *MAT_JOINTED_ROCK ◦ *MAT_SIMPLIFIED_RUBBER ◦ *MAT_FHWA_SOIL ◦ *MAT_SCHWER_MURRAY_CAP_MODEL • Failure time added to MAT_EROSION for solid elements. • Damping in the material models *MAT_LOW_DENSITY_FOAM and *MAT_- LOW_DENSITY_VISCOUS_FOAM can now be a tabulated function of the smallest stretch ratio. • The material model *MAT_PLASTICITY_WITH_DAMAGE allows the table definitions for strain rate. • Improvements in the option *INCLUDE_STAMPED_PART now allow all history data to be mapped to the crash part from the stamped part. Also, symmetry planes can be used to allow the use of a single stamping to initialize symmetric parts. • Extensive improvements in trimming result in much better elements after the trimming is completed. Also, trimming can be defined in either a local or global coordinate system. This is a new option in *DEFINE_CURVE_TRIM. • An option to move parts close before solving the contact problem is available, see *CONTACT_AUTO_MOVE. INTRODUCTION • An option to add or remove discrete beams during a calculation is available with the new keyword: *PART_SENSOR. • Multiple jetting is now available for the Hybrid and Chemkin airbag inflator models. • Nearly all constraint types are now handled for implicit solutions. • Calculation of constraint and attachment modes can be easily done by using the option: *CONTROL_IMPLICIT_MODES. • Penalty option, see *CONTROL_CONTACT, now applies to all *RIGIDWALL options and is always used when solving implicit problems. • Solid elements types 3 and 4, the 4 and 8 node elements with 6 degrees-of- freedom per node are available for implicit solutions. • The warping stiffness option for the Belytschko-Tsay shell is implemented for implicit solutions. The Belytschko-Wong-Chang shell element is now available for implicit applications. The full projection method is implemented due to it accuracy over the drill projection. • Rigid to deformable switching is implemented for implicit solutions. • Automatic switching can be used to switch between implicit and explicit calculations. See the keyword: *CONTROL_IMPLICIT_GENERAL. • Implicit dynamics rigid bodies are now implemented. See the keyword *CON- TROL_IMPLICIT_DYNAMIC. • Eigenvalue solutions can be intermittently calculated during a transient analysis. • A linear buckling option is implemented. See the new control input: *CON- TROL_IMPLICIT_BUCKLE • Implicit initialization can be used instead of dynamic relaxation. See the keyword *CONTROL_DYNAMIC_RELAXATION where the parameter, IDFLG, is set to 5. • Superelements, i.e., *ELEMENT_DIRECT_MATRIX_INPUT, are now available for implicit applications. • There is an extension of the option, *BOUNDARY_CYCLIC, to symmetry planes in the global Cartesian system. Also, automatic sorting of nodes on symmetry planes is now done by LS-DYNA. • Modeling of wheel-rail contact for railway applications is now available, see *RAIL_TRACK and *RAIL_TRAIN. • A new, reduced CPU, element formulation is available for vibration studies when elements are aligned with the global coordinate system. See *SECTION_- SOLID and *SECTION_SHELL formulation 98. • An option to provide approximately constant damping over a range of frequen- cies is implemented, see *DAMPING_FREQUENCY_RANGE. INTRODUCTION Features added during 2003-2005 for the 971 release of LS-DYNA: fully functional Initially, the intent was to quickly release version 971 after 970 with the implicit for distributed memory processing using MPI. capabilities Unfortunately, the effort required for parallel implicit was grossly underestimated, and, as a result, the release has been delayed. Because of the delay, version 971 has turned into a major release. Some of the new features, listed below, were also added to later releases of version 970. The new explicit capabilities are implemented in the MPP version and except for one case, in the SMP version as well. Below is list of new capabilities and features: • A simplified method for using the ALE capability with airbags is now available with the keyword *AIRBAG_ALE. • Case control using the *CASE keyword, which provides a way of running multiple load cases sequentially within a single run • New option to forming contact: *CONTACT_FORMING_ONE_WAY_SUR- FACE_TO_SURFACE_SMOOTH, which use fitted surface in contact calculation. • Butt weld definition by using the *CONSTRAINED_BUTT_WELD option which makes the definition of butt welds simple relative to the option: *CON- STRAINED_GENERALIZED_WELD_BUTT. • H-adaptive fusion is now possible as an option with the control input, *CON- TROL_ADAPTIVE. • Added a parameter on, *CONTROL_ADAPTIVE, to specify the number of elements generated around a 90 degree radius. A new option to better calculate the curvature was also implemented. • Added a new keyword: *CONTROL_ADAPTIVE_CURVE, to refine the element along trimming curves • Birth and death times for implicit dynamics on the keyword *CONTROL_IM- PLICIT_DYNAMICS. • Added an option to scale the spot weld failure resultants to account for the location of the weld on the segment surface, see *CONTROL_SPOTWELD_- BEAM. • Added an option which automatically replaces a single beam spot weld by an assembly of solid elements using the same ID as the beam that was replaced, see *CONTROL_SPOTWELD_BEAM. • Boundary constraint in a local coordinate system using *CONSTRAINED_LO- CAL keyword. • A cubic spline interpolation element is now available, *CONSTRAINED_- SPLINE. INTRODUCTION • Static implicit analyses in of a structure with rigid body modes is possible using the option, *CONTROL_IMPLICIT_INERTIA_RELIEF. • Shell element thickness updates can now be limited to part ID’s within a specified set ID, see the *CONTROL_SHELL keyword. The thickness update for shells can now be optionally limited to the plastic part of the strain tensor for better stability in crash analysis. • Solid element stresses in spot welds are optionally output in the local system using the SWLOCL parameter on the *CONTROL_SOLID keyword. • SPOTHIN option on the *CONTROL_CONTACT keyword cards locally thins the spot welded parts to prevent premature breakage of the weld by the contact treatments. • New function: *CONTROL_FORMING_PROJECT, which can initial move the penetrating slave nodes to the master surface • New function *CONTROL_FORMING_TEMPLATE, which allows user to easily set up input deck. Its function includes auto-position, define travel curve, termi- nation time, and most of the forming parameters for most of the typical forming process. • New function *CONTROL_FORMING_USER, *CONTROL_FORMING_POSI- TION, and *CONTROL_FORMING_TRAVEL, when used together, can allow the user to define atypical forming process. • Added new contact type *CONTACT_GUIDED_CABLE. • Circular cut planes are available for *DATABASE_CROSS_SECTION definitions. • New binary database FSIFOR for fluid structure coupling. • Added *DATABASE_BINARY_D3PROP for writing the material and property data to the first D3PLOT file or to a new database D3PROP. • DATABASE_EXTENT_BINARY has new flags to output peak pressure, surface energy density, nodal mass increase from mass scaling, thermal fluxes, and temperatures at the outer surfaces of the thermal shell. • Eight-character alphanumeric labels can now be used for the parameters SECID, MID, EOSID, HGID, and TMID on the *PART keyword. • Two NODOUT files are now written: one for high frequency output and a second for low frequency output. • Nodal mass scaling information can now be optionally written to the D3PLOT file. • Added option, MASS_PROPERTIES, to include the mass and inertial properties in the GLSTAT and SSSTAT files. • Added option in *CONTROL_CPU to output the cpu and elapsed time into the GLSTAT file. INTRODUCTION • Added an option, IERODE, on the *CONTROL_OUTPUT keyword to include eroded energies by part ID into the MATSUM file. Lumped mass kinetic energy is also in the MATSUM file as part ID 0. • Added an option, TET10, on the *CONTROL_OUTPUT keyword to output ten connectivity nodes into D3PLOT database rather than 4. • New keyword, *ELEMENT_SOLID_T4TOT10 to convert 4 node tetrahedron elements to 10 node tetrahedron elements. • New keyword, *ELEMENT_MASS_PART defines the total additional non- structural mass to be distributed by an area weighted distribution to all nodes of a given part ID. • New keyword option, SET, for *INTIAL_STRESS_SHELL_SET allows a set of shells to be initialized with the state of stress. • New option allows the number of cpu’s to be specified on the *KEYWORD input. • Tubular drawbead box option for defining the elements that are included in the drawbead contact, see *DEFINE_BOX_DRAWBEAD. • New function: *DEFINE_CURVE_DRAWBEAD, allow user to conveniently define drawbead by using curves (in x, y format or iges format) • New function: *DEFINE_DRAWBEAD_BEAM, which allows user to convenient- ly define drawbead by using beam part ID, and specify the drawbead force. • Analytic function can be used in place of load curves with the option *DEFINE_- CURVE_FUNCTION. • Friction can now be defined between part pair using the *DEFINE_FRICTION input. • New keyword: *DEFINE_CURVE_TRIM_3D, to allow trimming happens based on blank element normal, rather than use pre-defined direction • A new trimming algorithm was added: *DEFINE_CURVE_TRIM_NEW, which allow seed node to be input and is much faster then the original algorithm. • A new keyword, *DEFINE_HEX_SPOTWELD_ASSEMBLY, is available to define a cluster of solid elements that comprise a single spot weld. • The definition of a vector, see *DEFINE_VECTOR, can be done by defining coordinates in a local coordinate system. • The definition of a failure criteria between part pairs is possible with a table defined using the keyword, *DEFINE_SPOTWELD_FAILURE_RESULTANTS. • A new keyword, *DEFINE_CONNECTION_PROPERTIES is available for defining failure properties of spot welds. • Added *DEFINE_SET_ADAPTIVE to allow the adaptive level and element size to be specified by part ID or element set ID. INTRODUCTION • Static rupture stresses for beam type spot welds can be defined in the keyword input, *DEFINE_SPOTWELD_RUPTURE_STRESS. • Section properties can be define in the *ELEMENT_BEAM definitions for resultant beam elements using the SECTION option. • Physical offsets of the shell reference surface can be specified on the shell element cards, see the OFFSET option on *ELEMENT_SHELL. • File names can be located in remote directories and accessed through the *IN- CLUDE_PART keyword. • New features to *INCLUDE_STAMPED_PART: two different mirror options, user-defined searching radius. • *INTIAL_STRESS_SECTION allows for stress initialization across a cross-section, which consists of solid elements. • An option, IVATN, is available for setting the velocities of slaved nodes and parts for keyword, *INITIAL_VELOCITY_GENERATION. • Twenty-two built-in cross-section are now available in the definition of beam integration rules, see *INTEGRATION_BEAM. • The possibility of changing material types is now available for shells using the user defined integration rule, see *INTEGRATION_SHELL. • The interface springback file created by using the keyword, *INTERFACE_- SPRINGBACK is now optionally written as a binary file. • An optional input line for *KEYWORD allows the definition of a prefix for all file names created during a simulation. This allows multiple jobs to be executed in the same directory. • Body force loads can now be applied in a local coordinate system for *LOAD_- BODY. • A pressure loading feature allows moving pressures to be applied to a surface to simulate spraying a surface with stream of fluid through a nozzle. See keyword *LOAD_MOVING_PRESSURE. • Thermal expansion can be added to any material by the keyword, *MAT_ADD_- THERMAL_EXPANSION. • Curves can now be used instead of eight digitized data points in the material model *MAT_ELASTIC_WITH_VISCOSITY_CURVE • New options for spot weld failure in *MAT_SPOTWELD, which apply to beam and solid elements. • Failure criteria based on plastic strain to failure is added to material *MAT_- ANISOTROPIC_VISCOPLASTIC. • Strain rate failure criterion is added to material *MAT_MODIFIED_PIECE- WISE_LINEAR_PLASTICITY. INTRODUCTION • Strain rate scaling of the yield stress can now be done differently in tension and compression in material with separate pressure cut-offs in tension and compres- sion in material model *MAT_PLASTICITY_TENSION_COMPRESSION. • The RCDC model is now available to predict failure in material *MAT_PLASTIC- ITY_WITH_DAMAGE. • Two additional yield surfaces have been added to material *MAT_MODIFIED_- HONEYCOMB to provide more accurate predictions of the behavior of honey- comb barrier models. • Unique coordinate systems can be assigned to the two nodal points of material *MAT_1DOF_GENERALIZED_SPRING. • Poisson’s ratio effects are available in foam defined by load curves in the material *MAT_SIMPLIFIED_RUBBER/FOAM • Failure effects are available in the rubber/foam material defined by load curves in the *MAT_SIMPLIFIED_RUBBER/FOAM_WITH_FAILURE. • The material option *MAT_ADD_EROSION now allows the maximum pressure at failure and the minimum principal strain at failure to be specified. • Strains rather than displacements can now be used with the material model for discrete beams, *MAT_GENERAL_NONLINEAR_6DOF_DISCRETE_BEAM. • New option for *MAT_TRANSVERSELY_ANISOTROPIC_ELASTIC_PLAS- TIC_(ECHANGE), which allow two ways to change the Young’s modulus dur- ing forming simulation. • New Material model: *MAT_HILL_3R: includes the shear term in the yield surface calculation by using Hill’s 1948 an-isotropic material model. • New Material model: *MAT_KINEMATIC_HARDENING_TRANSVERSELY_- ANISOTROPIC: which integrates Mat #37 with Yoshida’s two-surface kinematic hardening model. • Improved formulation for the fabric material, *MAT_FABRIC for formulations 2, 3, and 4. The improved formulations are types 12, 13, and 14. • Constitutive models added for truss elements: ◦ *MAT_MUSCLE • For beam elements ◦ *MAT_MOMENT_CURVATURE • For shell elements ◦ *MAT_RESULTANT_ANISOTROPIC ◦ *MAT_RATE_SENSITIVE_COMPOSITE_FABRIC. ◦ *MAT_SAMP-1 INTRODUCTION ◦ *MAT_SHAPE_MEMORY is now implemented for shells. • for shell and solid elements: ◦ *MAT_BARLAT_YLD2000 for anisotropic aluminum alloys. ◦ *MAT_SIMPLIFIED_RUBBER_WITH_DAMAGE ◦ *MAT_VISCOELASTIC_THERMAL ◦ *MAT_THERMO_ELASTO_VISCOPLASTIC_CREEP • for the solid elements: ◦ *MAT_ARUP_ADHESIVE ◦ *MAT_BRAIN_LINEAR_VISCOELASTIC. ◦ *MAT_CSCM for modeling concrete. ◦ *MAT_PLASTICITY_COMPRESSION_TENSION_EOS for modeling ice. ◦ *MAT_COHESIVE_ELASTIC ◦ *MAT_COHESIVE_TH ◦ *MAT_COHESIVE_GENERAL ◦ *MAT_EOS_GASKET ◦ *MAT_SIMPLIFIED_JOHNSON_COOK is now implemented for solids. ◦ *MAT_PLASTICITY_WITH_DAMAGE is now implemented for solids. ◦ *MAT_SPOTWELD_DAIMLERCHRYSLER • User defined equations-of-state are now available. • There is now an interface with the MOLDFLOW code. • Damping defined in *DAMPING_PART_STIFFNESS now works for the Belytschko –Schwer beam element. • The option *NODE_TRANSFORMATION allows a node set to be transformed based on a transformation defined in *DEFINE_TRANSFORMATION. • Parameters can be defined in FORTRAN like expressions using *PARAMETER_- EXPRESSION. • A part can be moved in a local coordinate system in *PART_MOVE. • A simplified method for defining composite layups is available with *PART_- COMPOSITE • The rigid body inertia can be changed in restart via *CHANGE_RIGID_BODY_- INERTIA. • A part set can now be defined by combining other part sets in *SET_PART_ADD. • Termination of the calculation is now possible if a specified number of shell elements are deleted in a give part ID. See *TERMINATION_DELETED_- SHELLS. INTRODUCTION • Added hourglass control type 7 for solid elements for use when modeling hyperelastic materials. • Shell formulations 4, 11, 16, and 17 can now model rubber materials. • Added a new seatbelt pretensioner type 7 in which the pretensioner and retractor forces are calculated independently and added. • A new composite tetrahedron element made up from 12 tetrahedron is now available as solid element type 17. • Shell thickness offsets for *SECTION_SHELL now works for most shell elements, not just the Hughes-Liu shell. • The Hughes-Liu beam has been extended to include warpage for open cross- sections. • A resultant beam formulation with warpage is available as beam type 12. • Two nonlinear shell elements are available with 8 degrees-of-freedom per node to include thickness stretch. • Tetrahedron type 13, which uses nodal pressures, is now implemented for implicit applications. • Cohesive solid elements are now available for treating failure. • Seatbelt shell elements are available for use with the all seatbelt capabilities. • Superelements can now share degrees-of-freedom and are implemented for implicit applications under MPI. • A user defined element interface is available for solid and shell elements. • Thermal shells are available for treating heat flow through shell elements. • EFG shell formulations 41 and 42 are implemented for explicit analysis. • EFGPACK is implemented in addition to BCSLIB-EXT solver on the keyword *CONTROL_EFG. • EFG MPP version is available for explicit analysis. • EFG fast transformation method is implemented in the EFG solid formulation. • EFG Semi-Lagrangian kernel and Eulerian kernel options are added for the foam materials. • EFG 3D adaptivity is implemented for the metal materials. • EFG E.O.S. and *MAT_ELASTIC_FLUID materials are included in the 4-noded background element formulation. • Airbag simulations by using ALE method can be switched to control volume method by *ALE_CV_SWITCH. • *MAT_ALE_VISCOUS now supports Non-Newtonian viscosity by power law or load curve. INTRODUCTION • *DATABASE_BINARY_FSIFOR outputs fluid-structure interaction data to binary file. • *DATABASE_FSI_SENSOR outputs ALE element pressure to ASCII file dbsor. • *MAT_GAS_MIXTURE supports nonlinear heat capacities. • *INITIAL_VOLUME_FRACTION_GEOMETRY uses an enhanced algorithm to handle both concave and convex geometries and substantially reduce run time. • A new keyword *DELETE_FSI allows the deletion of coupling definitions. • Convection heat transfer activates by *LOAD_ALE_CONVECTION in ALE FSI analysis. • *ALE_FSI_SWITCH_MMG is implemented to switch between ALE multi- material groups to treat immersed FSI problems. • Type 9 option is added in *ALE_REFERENCE_SYSTEM_GROUP to deal complex ALE mesh motions including translation, rotation, expansion and contraction, etc. ◦ New options in *CONSTRAINED_LAGRANGE_IN_SOLID ◦ Shell thickness option for coupling type 4. ◦ Bulk modulus based coupling stiffness. ◦ Shell erosion treatment. ◦ Enable/disable interface force file. • New coupling method for fluid flowing through porous media are implemented as type 11 (shell) and type 12 (solid) in *CONSTRAINED_LAGRANGE_IN_SOL- ID. • *ALE_MODIFIED_STRAIN allows multiple strain fields in certain ALE elements to solve sticking behavior in FSI. (MPP underdevelopment) • *ALE_FSI_PROJECTION is added as a new constraint coupling method to solve small pressure variation problem. (MPP underdevelopment) • *BOUNDARY_PRESCRIBED_ORIENTATION_RIGID is added as a means to prescribe as a function of time the general orientation of a rigid body using a variety of methods. This feature is available in release R3 and higher of Version 971. • *BOUNDARY_PRESCRIBED_ACCELEROMETER_RIGID is added as a means to prescribe the motion of a rigid body based un experimental data gathered from accelerometers affixed to the rigid body. This feature is available in release R3 and higher of Version 971. INTRODUCTION Capabilities added during 2008-2011 for Version 971R6 of LS-DYNA: During the last four years the implicit capabilities are now scalable to a large number of cores; therefore, LS-DYNA has achieved a major goal over 15 years of embedding a scalable implicit solver. Also, in addition to the progress made for implicit solutions many other new and useful capabilities are now available. • The keyword *ALE_AMBIENT_HYDROSTATIC initializes the hydrostatic pressure field in the ambient ALE domain due to an acceleration like gravity. • The keyword *ALE_FAIL_SWITCH_MMG allows switching an ALE multi- material-group ID (AMMGID) if the material failure criteria occurs. • The keyword *ALE_FRAGMENTATION allow switching from the ALE multi- material-group ID, AMMGID, (FR_MMG) of this failed material to another AM- MGID (TO_MMG). This feature may typically be used in simulating fragmenta- tion of materials. • The keyword *ALE_REFINE refines ALE hexahedral solid elements automatical- ly. • The keyword *BOUNDARY_ALE_MAPPING maps ALE data histories from a previous run to a region of elements. Data are read from or written to a map- ping file with a file name given by the prompt “map=” on the command line starting the execution. • The keyword *BOUNDARY_PORE_FLUID is used to define parts that contain pore fluid where defaults are given on *CONTROL_PORE_FLUID input. • With the keyword, *BOUNDARY_PRESCRIBED_FINAL_GEOMETRY, the final displaced geometry for a subset of nodal points is defined. The nodes of this subset are displaced from their initial positions specified in the *NODE input to the final geometry along a straight line trajectory. A load curve defines a scale factor as a function of time that is bounded between zero and unity correspond- ing to the initial and final geometry, respectively. A unique load curve can be specified for each node, or a default load curve can apply to all nodes. • The keyword, *BOUNDARY_PWP, defines pressure boundary conditions for pore water at the surface of the software. • The keyword, *CONSTRAINED_JOINT_COOR, defines a joint between two rigid bodies. The connection coordinates are given instead of the nodal point IDs used in *CONSTRAINED_JOINT. • The keyword, *CONSTRAINED_SPR2, defines a self-piercing rivet with failure. This model for a self-piercing rivet (SPR2) includes a plastic-like damage model that reduces the force and moment resultants to zero as the rivet fails. The domain of influence is specified by a diameter, which should be approximately equal to the rivet’s diameter. The location of the rivet is defined by a single node at the center of two riveted sheets. INTRODUCTION • Through the keyword, *CONTROL_BULK_VISCOSITY, bulk viscosity is optional for the Hughes-Liu beam and beam type 11 with warpage. This option often provides better stability, especially in elastic response problems. • The display of nodal rigid bodies is activated by the parameter, PLOTEL, on the *CONTROL_RIGID keyword. • The mortar contact, invoked by appending the suffix MORTAR to either FORM- ING_SURFACE_TO_SURFACE, AUTOMATIC_SURFACE_TO_SURFACE or AUTOMATIC_SINGLE_SURFACE, is a segment to segment penalty based contact. For two segments on each side of the contact interface that are overlap- ping and penetrating, a consistent nodal force assembly taking into account the individual shape functions of the segments is performed. In this respect the results with this contact may be more accurate, especially when considering contact with elements of higher order. By appending the suffix TIED to the CONTACT_AUTOMATIC_SURFACE_TO_SURFACE_MORTAR keyword or the suffix MORTAR to the CONTACT_AUTOMATIC_SURFACE_TO_SUR- FACE_TIEBREAK keyword, this is treated as a tied contact interface with tie- break failure in the latter case. Only OPTION = 9 is supported for the mortar tiebreak contact. The mortar contact is intended for implicit analysis in particu- lar but is nevertheless supported for explicit analysis as well. • In the database, ELOUT, the number of history variables can be specified for output each integration point in the solid, shell, thick shell, and beam elements. The number of variables is given on the *DATABASE_ELOUT keyword defini- tion. • A new option is available in *DATABASE_EXTENT_BINARY. Until now only one set of integration points were output through the shell thickness. The lamina stresses and history variables were averaged for fully integrated shell elements, which results in less disk space for the D3PLOT family of files, but makes it difficult to verify the accuracy of the stress calculation after averaging. An option is now available to output all integration point stresses in fully inte- grated shell elements: 4 x # of through thickness integration points in shell types 6, 7, 16, 18-21, and 3 x # of through thickness integration points in triangular shell types 3, and 17. • The keyword *DATABASE_PROFILE allows plotting the distribution or profile of data along x, y, or z-direction. • The purpose of the keyword, *DEFINE_ADAPTIVE_SOLID_TO_SPH, is to adaptively transform a Lagrangian solid Part or Part Set to SPH particles when the Lagrange solid elements comprising those parts fail. One or more SPH particles (elements) will be generated for each failed element to. The SPH parti- cles replacing the failed element inherit all of the properties of failed solid ele- ment, e.g. mass, kinematic variables, and constitutive properties. INTRODUCTION • With the keywords beginning with, *DEFINE_BOX, a LOCAL option is now available. With this option the diagonal corner coordinates are given in a local coordinate system defined by an origin and vector pair. • The keyword, *DEFINE_CURVE_DUPLICATE, defines a curve by optionally scaling and offsetting the abscissa and ordinates of another curve defined by the *DEFINE_CURVE keyword. • The keyword, *DEFINE_ELEMENT_DEATH, is available to delete a single element or an element set at a specified time during the calculation. • The purpose of the keyword, *DEFINE_FRICTION_ORIENTATION, is to allow for the definition of different coefficients of friction (COF) in specific directions, specified using a vector and angles in degrees. In addition, COF can be scaled according to the amount of pressure generated in the contact interface. • With the new keyword, *DEFINE_FUNCTION, an arithmetic expression involving a combination of independent variables and other functions, i.e., f(a,b,c) = a*2 + b*c + sqrt(a*c) is defined where a, b, and c are the independent variables. This option is im- plemented for a subset of keywords. ◦ *ELEMENT_SEATBELT_SLIPRING ◦ *LOAD_BEAM ◦ *LOAD_MOTION_NODE ◦ *LOAD_MOVING_PRESSURE ◦ *LOAD_NODE ◦ *LOAD_SEGMENT ◦ *LOAD_SEGMENT_NONUNIFORM ◦ *LOAD_SETMENT_SET_NONUNIFORM ◦ *BOUNDARY_PRESCRIBED_MOTION • If a curve ID is not found, then the function ID’s are checked. • The keyword, *DEFINE_SPH_TO_SPH_COUPLING, defines a penalty based contact to be used for the node to node contacts between SPH parts. • The keyword, *DEFINE_TABLE_2D, permits the same curve ID to be referenced by multiple tables, and the curves may be defined anywhere in the input. • The keyword, *DEFINE_TABLE_3D, provides a way of defining a three- dimensional table. A 2D table ID is specified for each abscissa value defined for the 3D table. • The keyword, *ELEMENT_BEAM_PULLEY, allows the definition of a pulley for truss beam elements . Currently, the beam pulley is implemented for *MAT_001 and *MAT_156. Pulleys allow continuous sliding of a string of truss beam element through a sharp change of angle. INTRODUCTION • The purpose of the keyword, *ELEMENT_MASS_MATRIX, is to define a 6x6 symmetric nodal mass matrix assigned to a nodal point or each node within a node set. • The keyword, *ELEMENT_DISCRETE_SPHERE, allows the definition of a discrete spherical element for discrete element calculations. Each particle con- sists of a single node with its mass, mass moment of inertia, and radius. Initial coordinates and velocities are specified via the nodal data. • The two keywords, *ELEMENT_SHELL_COMPOSITE and *ELEMENT_- TSHELL_COMPOSITE, are used to define elements for a general composite shell part where the shells within the part can have an arbitrary number of layers. The material ID, thickness, and material angle are specified for the thickness integra- tion points for each shell in the part • The keyword, *EOS_USER_DEFINED, allows a user to supply their own equation-of-state subroutine. • The new keyword *FREQUENCY_DOMAIN provides a way of defining and solving frequency domain vibration and acoustic problems. The related key- word cards given in alphabetical order are: ◦ *FREQUENCY_DOMAIN_ACOUSTIC_BEM_{OPTION} ◦ *FREQUENCY_DOMAIN_ACOUSTIC_FEM ◦ *FREQUENCY_DOMAIN_FRF ◦ *FREQUENCY_DOMAIN_RANDOM_VIBRATION ◦ *FREQUENCY_DOMAIN_RESPONSE_SPECTRUM ◦ *FREQUENCY_DOMAIN_SSD • The keyword, *INITIAL_AIRBAG_PARTICLE, initializes pressure in a closed airbag volume, door cavities for pressure sensing studies, and tires. • The keyword *INITIAL_ALE_HYDROSTATIC initializes the hydrostatic pressure field in an ALE domain due to an acceleration like gravity. • The keyword *INITIAL_ALE_MAPPING maps ALE data histories from a previous run. Data are read from a mapping file with a file name given by the prompt “map=” on the command line starting the execution. • The keyword, *INITIAL_AXIAL_FORCE_BEAM, provides a simplified method to model initial tensile forces in bolts. • The keyword, *INITIAL_FIELD_SOLID, is a simplified version of the *INITIAL_- STRESS_SOLID keyword which can be used with hyperelastic materials. This keyword is used for history variable input. Data is usually in the form of the eigenvalues of diffusion tensor data. These are expressed in the global coordi- nate system. • The equation-of-state, *EOS_MIE_GRUNEISEN, type 16, is a Mie-Gruneisen form with a p-α compaction model. INTRODUCTION • The keyword, *LOAD_BLAST_ENHANCED, defines an air blast function for the application of pressure loads due the explosion of conventional charge. While similar to *LOAD_BLAST this feature includes enhancements for treating reflect- ed waves, moving warheads and multiple blast sources. The loads are applied to facets defined with the keyword *LOAD_BLAST_SEGMENT. A database con- taining blast pressure history is also available . • The keyword, *LOAD_ERODING_PART_SET, creates pressure loads on the exposed surface composed of solid elements that erode, i.e., pressure loads are added to newly exposed surface segments as solid elements erode. • The keyword, *LOAD_SEGMENT_SET_ANGLE, applies traction loads over a segment set that is dependent on the orientation of a vector. An example appli- cation is applying a pressure to a cylinder as a function of the crank angle in an automobile engine • The keyword, *LOAD_STEADY_STATE_ROLLING, is a generalization of *LOAD_BODY, allowing the user to apply body loads to part sets due to transla- tional and rotational accelerations in a manner that is more general than the *LOAD_BODY capability. The *LOAD_STEADY_STATE_ROLLING keyword may be invoked an arbitrary number of times in the problem as long as no part has the option applied more than once and they can be applied to arbitrary meshes. This option is frequently used to initialize stresses in tire. • The keywords INTERFACE_SSI, INTERFACE_SSI_AUX, INTERFACE_SSI_- AUX_EMBEDDED and INTERFACE_SSI_STATIC are used to define the soil- structure interface appropriately in various stages of soil-structure interaction analysis under earthquake ground motion. • The keyword, *LOAD_SEISMIC_SSI, is used to apply earthquake loads due to free-field earthquake ground motion at certain locations — defined by either nodes or coordinates — on a soil-structure interface. This loading is used in earthquake soil-structure interaction analysis. The specified motions are used to compute a set of effective forces in the soil elements adjacent to the soil-structure interface, according to the effective seismic input–domain reduction method. • The keyword *DEFINE_GROUND_MOTION is used to specify a ground motion to be used in conjunction with *LOAD_SEISMIC_SSI. • Material types *MAT_005 and *MAT_057 now accept table input to allow the stress quantity versus the strain measure to be defined as a function of tempera- ture. • The material option *MAT_ADD_EROSION, can now be applied to all nonlinear shell, thick shell, fully integrated solids, and 2D solids. New failure criteria are available. • The GISSMO damage model, now available as an option in *MAT_ADD_ERO- SION, is a phenomenological formulation that allows for an incremental descrip- INTRODUCTION tion of damage accumulation, including softening and failure. It is intended to provide a maximum in variability for the description of damage for a variety of metallic materials (e.g. *MAT_024, *MAT_036, …). The input of parameters is based on tabulated data, allowing the user to directly convert test data to numer- ical input. • The keyword, *MAT_RIGID_DISCRETE or MAT_220, eliminates the need to define a unique rigid body for each particle when modeling a large number of rigid particles. This gives a large reduction in memory and wall clock time over separate rigid bodies. A single rigid material is defined which contains multiple disjoint pieces. Input is simple and unchanged, since all disjoint rigid pieces are identified automatically during initialization. • The keyword, *NODE_MERGE, causes nodes with identical coordinates to be replaced during the input phase by the node encountered that has the smallest ID. • The keyword, *PART_ANNEAL, is used to initialize the stress states at integra- tion points within a specified part to zero at a given time during the calculation. This option is valid for parts that use constitutive models where the stress is incrementally updated. This option also applies to the Hughes-Liu beam ele- ments, the integrated shell elements, thick shell elements, and solid elements. • The keyword, *PART_DUPLICATE, provides a method of duplicating parts or part sets without the need to use the *INCLUDE_TRANSFORM option. • To automatically generate elements to visualize rigid walls the DISPLAY option is now available for *RIGIDWALL_PLANAR and *RIGIDWALL_GEOMETRIC. • A one point integrated pentahedron solid element with hourglass control is implemented as element type 115 and can be referenced in *SECTION_SOLID. Also, the 2 point pentahedron solid, type 15, no longer has a singular mode. • The keyword *SECTION_ALE1D defines section properties for 1D ALE elements. • The keyword *SECTION_ALE2D defines section properties for 2D ALE elements. • The keywords *SET_BEAM_INTERSECT, *SET_SHELL_INTERSECT, *SET_SOL- ID_INTERSECT, *SET_NODE_INTERSECT, and *SET_SEGMENT_INTER-SECT, allows the definition of a set as the intersection, ∩, of a series of sets. The new set, SID, contains all common members. • The keyword, *SET_SEGMENT_ADD, is now available for defining a new segment set by combining other segment sets. • The two keywords, *DEFINE_ELEMENT_GENERALIZED_SHELL and *DE- FINE_ ELEMENT_GENERALIZED_SOLID, are used to define general shell and solid element formulations to allow the rapid prototyping of new element formula- INTRODUCTION tions. They are used in combination with the new keywords *ELEMENT_GEN- ERLIZED_SHELL and *ELEMENT_GENERALIZED_SOLID. • The two keywords, *ELEMENT_INTERPOLATION_SHELL and *ELEMENT_ INTERPOLATION_SOLID, are used to interpolate stresses and other solution variables from the generalized shell and solid element formulations for visualiza- tion. They are used together with the new keyword *CONSTRAINED_NODE_- INTERPOLATION. • The keyword, *ELEMENT_SHELL_NURBS_PATCH, is used to define 3D shell elements based on NURBS (Non-Uniform Ration B-Spline) basis functions. Currently four different element formulations, with and without rotational degrees of freedom are available. • The keyword LOAD_SPCFORC is used to apply equivalent SPC loads, read in from the d3dump file during a full-deck restart, in place of the original con- straints in order to facilitate the classical non-reflecting boundary on an outside surface. Capabilities added in 2012 to create Version 97R6.1, of LS-DYNA: • A new keyword *MAT_THERMAL_DISCRETE_BEAM defines thermal properties for ELFORM 6 beam elements. • An option *CONTROL_THERMAL_SOLVER, invoked by TSF < 0, gives the thermal speedup factor via a curve. This feature is useful when artificially scaling velocity in metal forming. • A nonlinear form of Darcy's law in *MAT_ADD_PORE_AIR allows curves to define the relationship between pore air flow velocity and pore air pressure gradient. • An extention to the PART option in *SET_SEGMENT_GENERAL allows reference to a beam part. This allows for creation of 2D segments for traction application. • Options “SET_SHELL”, “SET_SOLID”, “SET_BEAM”, “SET_TSHELL”, “SET_- SPRING” are added to *SET_NODE_GENERAL so users can define a node set using existing element sets. • Options “SET_SHELL”, “SET_SOLID”, “SET_SLDIO”, “SET_TSHELL”, “SET_- TSHIO” are added to *SET_SEGMENT_GENERAL so users can use existing element sets to define a segment set. • *BOUNDARY_PRESCRIBED_MOTION_SET_BOX prescribes motion to nodes that fall inside a defined box. • IPNINT > 1 in *CONTROL_OUTPUT causes d3hsp to list the IPNINT smallest element timesteps in ascending order. • Section and material titles are echoed to d3hsp. INTRODUCTION • A new parameter MOARFL in *DEFINE_CONNECTION_PROPERTIES permits reduction in modeled area due to shear. • A new option HALF_SPACE in *FREQUENCY_DOMAIN_ACOUSTIC_BEM enables treatment of a half-space in boundary element method, frequency do- main acoustic analysis. • A shell script “kill_by_pid” is created during MPP startup. When executed, this script will run “kill -9” on every LS-DYNA process started as part of the MPP job. This is for use at the end of submission scripts, as a “fail safe” cleanup in case the job aborts. • A new parameter IAVIS in *CONTROL_SPH selects the artificial viscosity formulation for the SPH particles. If set to 0, the Monaghan type artificial viscos- ity formulation is used. If set to 1, the standard artificial viscosity formulation for solid elements is used which may provide a better energy balance but is less stable in specific applications such as high velocity impact. • Contact friction may be included in *CONTACT_2D_NODE_TO_SOLID for SPH. • A new keyword *ALE_COUPLING_NODAL_CONSTRAINT provides a coupling mechanism between ALE solids and non-ALE nodes. The nodes can be from virtually any non-ALE element type including DISCRETE_SPHERE, EFG, and SPH, as well as the standard Lagrangian element types. In many cases, this coupling type may be a better alternative to *CONSTRAINED_LAGRANGE_- IN_SOLID. • The keyword *ALE_ESSENTIAL_BOUNDARY assigns essential boundary conditions to nodes of the ALE boundary surface. The command can be repeat- ed multiple times and is recommended over use of EBC in *CONTROL_ALE.. • The keyword *DELETE_ALECPL in a small restart deck deletes coupling defined with *ALE_COUPLING_NODAL_CONSTRAINT. The command can also be used to reinstate the coupling in a later restart. • *DEFINE_VECTOR_NODES defines a vector with two node points. • *CONTACT_AUTOMATIC_SINGLE_SURFACE_TIED allows for the calculation of eigenvalues and eigenvectors for models that include *CONTACT_AUTO- MATIC_SINGLE_SURFACE. • A new parameter RBSMS in *CONTROL_RIGID affects rigid body treatment in Selective Mass Scaling (*CONTROL_TIMESTEP). When rigid bodies are in any manner connected to deformable elements, RBSMS = 0 (default) results in spuri- ous inertia due to improper treatment of the nodes at the interface. RBSMS = 1 alleviates this effect but an additional cost is incurred. • A new parameter T10JTOL in *CONTROL_SOLID sets a tolerance for issuing a warning when J_min/J_max goes below this tolerance value (i.e., quotient between minimum and maximum Jacobian value in the integration points) for INTRODUCTION tetrahedron type 16. This quotient serves as an indicator of poor tetrahedral element meshes in implicit that might cause convergence problems. • A new option MISMATCH for *BOUNDARY_ACOUSTIC_COUPLING handles coupling of structural element faces and acoustic volume elements (ELFORMs 8 and 14) in the case where the coupling surfaces do not have coincident nodes. • A porosity leakage formulation in *MAT_FABRIC (*MAT_034, FLC < 0) is now available for particle gas airbags (*AIRBAG_PARTICLE). • *BOUNDARY_PRESCRIBED_ACCELEROMETER is disabled during dynamic relaxation. • A new parameter CVRPER in *BOUNDARY_PAP defines porosity of a cover material encasing a solid part. • A parameter TIEDID in *CONTACT_TIED_SURFACE_TO_SURFACE offers an optional incremental normal update in SMP to eliminate spurious contact forces that may appear in some applications. • A new option SPOTSTP = 3 in *CONTROL_CONTACT retains spot welds even when the spot welds are not found by *CONTACT_SPOTWELD. • The SMP consistency option (ncpu < 0) now pertains to the ORTHO_FRICTION contact option. • Forces from *CONTACT_GUIDED_CABLE are now written to ncforc (both ASCII and binout). • Discrete beam materials 70, 71, 74, 94, 121 calculate axial force based on change in length. Output the change in length instead of zero axial relative displace- ment to ASCII file disbout (*DATABASE_DISBOUT). • *DATABASE_RCFORC_MOMENT is now supported in implicit. • After the first implicit step, the output of projected cpu and wall clock times is written and the termination time is echoed. • *DATABASE_MASSOUT is upgraded to include a summary table and to optionally add mass for nodes belonging to rigid bodies. • Generate and store resultant forces for the LaGrange Multiplier joint formulation so as to give correct output to jntforc (*DATABASE_JNTFORC). • Control the number of messages for deleted and failed elements using parameter MSGMAX in *CONTROL_OUTPUT. • Nodal and resultant force output is written to nodfor for nodes defined in *FREQUENCY_DOMAIN_SSD in *DATABASE_NODAL_FORCE_GROUP analysis (SMP only). • Ncforc data is now written for guided cables (*CONTACT_GUIDED_CABLE) in MPP. INTRODUCTION • Jobid handling is improved in l2a utility so that binout files from multiple jobs, with or without a jobid-prefix, can be converted with the single command “l2a -j *binout*”. The output contains the correct prefix according to the jobid. • ALE_MULTI-MATERIAL_GROUP (AMMG) info is written to matsum (both ASCII and binout). • Shell formulation 14 is switched to 15 (*SECTION_SHELL) in models that include axisymmetric SPH. • *ELEMENT_BEAM_PULLEY is permitted with *MAT_CABLE_DISCRETE_- BEAM. • A warning during initialization is written if a user creates DKT triangles, either by ELFORM = 17 on *SECTION_SHELL or ESORT = 2 on *CONTROL_SHELL, that are thicker than the maximum edge length. • Account is taken of degenerate acoustic elements with ELFORM 8. Tria and quad faces at acoustic-structure boundary are handled appropriately according to shape. • The compression elimination option for 2D seatbelts, CSE = 2 in *MAT_SEAT- BELT is improved. • Detailed material failure (*MAT_ADD_EROSION) messages in messag and d3hsp are suppressed when number of messages > MSGMAX (*CONTROL_- OUTPUT). • Implement SMP consistency (*MAT_186) solids and shells. (ncpu < 0) in *MAT_COHESIVE_GENERAL • Viscoelastic model in *MAT_077_O now allows up to twelve terms in Prony series instead of standard six. • Large curve ID's for friction table (*CONTACT_… with FS = 2) are enabled. • Efficiency of GISSMO damage in *MAT_ADD_EROSION is improved. • *MAT_ADD_PERMEABILITY_ORTHOTROPIC is now available for pore pressure analysis (*…_PORE_FLUID). • For *MAT_224 solids and shells, material damage serves as the failure variable in *CONSTRAINED_TIED_NODES_FAILURE. • The behavior of *MAT_ACOUSTIC is modified when used in combination with dynamic relaxation (DR). Acoustic domain now remains unperturbed in the DR phase but hydrostatic pressure from the acoustic domain is applied to the struc- ture during DR. • Option for 3D to 2D mapping is added in *INITIAL_ALE_MAPPING. • *CONTACT_ERODING_NODES_TO_SURFACE contact may be used with SPH particles. INTRODUCTION • Total Lagrangian SPH formulation 7 (*CONTROL_SPH) is now available in MPP. • The output formats for linear equation solver statistics now accommodate very large numbers as seen in large models. • *CONTROL_OUTPUT keyword parameter NPOPT is now applicable to thermal data. If NPOPT = 1, then printing of the following input data to d3hsp is sup- pressed: ◦ *INITIAL_TEMPERATURE ◦ *BOUNDARY_TEMPERATURE ◦ *BOUNDARY_FLUX ◦ *BOUNDARY_CONVECTION ◦ *BOUNDARY_RADIATION ◦ *BOUNDARY_ENCLOSURE_RADIATION • Beam energy balance information is written to TPRINT file. • MPP performance for LS-DYNA/Madymo coupling is improved. • Shell adaptivity (*CONTROL_ADAPTIVE) is improved to reduce the number of elements along curved surfaces in forming simulations. • One-step unfolding (*CONTROL_FORMING_ONESTEP) is improved to accommodate blanks with small initial holes. • Efficiency of FORM 3 isogeometric shells is improved. • The processing of *SET_xxx_GENERAL is faster. • *KEYWORD_JOBID now works even when using the *CASE command. • Parts may be repositioned in a small restart by including *DEFINE_TRANSFOR- MATION and *NODE_TRANSFORM in the small restart deck to move nodes of a specified node set prior to continuing the simulation. Capabilities added during 2012/2013 to create LS-DYNA R7.0: • Three solvers, EM, CESE, and ICFD, and a volume mesher to support the latter two solvers, are new in Version 7. Brief descriptions of those solvers are given below. Keyword commands for the new solvers are in Volume III of the LS- DYNA Keyword User’s Manual. These new solvers are only included in double precision executables. • Keyword family: *EM_, the keywords starting with *EM refer to and control the Electromagnetic solver problem set up: ◦ EM Solver Characteristics: Implicit INTRODUCTION Double precision Dynamic memory handling SMP and MPP 2D axisymmetric solver / 3D solver Automatic coupling with structural and thermal LS-DYNA solvers FEM for conducting pieces only, no air mesh needed (FEM-BEM sys- tem) Solid elements for conductors, shells can be insulators ◦ EM Solver Main Features: Eddy Current (a.k.a Induction-Diffusion) solver Induced heating solver Resistive heating solver Imposed tension or current circuits Exterior field Magnetic materials (beta version) Electromagnetic contact EM Equation of states (Conductivity as a function of temperature) ◦ EM Solver Applications (Non-exhaustive) : Electromagnetic forming Electromagnetic welding Electromagnetic bending Inductive heating Resistive heating Rail-gun Ring expansions • Keyword family: *CESE_, the keywords starting with *CESE refer to and control the Compressible CFD solver problem set up: ◦ CESE Solver Characteristics: Explicit Double precision Dynamic memory handling SMP and MPP 3D solver / special case 2D solver and 2D axisymmetric solver Automatic coupling with structural and thermal LS-DYNA solvers Eulerian fixed mesh or moving mesh (Either type input with *ELE- MENT_SOLID cards or using *MESH cards) ◦ CESE Solver Main Features: INTRODUCTION The CESE (Conservation Element / Solution Element) method en- forces conservation in space-time Highly accurate shock wave capturing Cavitation model Embedded (immersed) boundary approach or moving (fitting) ap- proach for FSI problems Coupled stochastic fuel spray solver Coupling with chemistry solver ◦ CESE Solver Applications (Non-exhaustive) : Shock wave capturing Shock/acoustic wave interaction Cavitating flows Conjugate heat transfer problems Many different kinds of stochastic particle flows, e.g, dust, water, fuel. Chemically reacting flows, e.g, detonating flow, supersonic combus- tion. • Keyword family: *ICFD_, the keywords starting with *ICFD refer to and control the incompressible CFD solver problem set up: ◦ ICFD Solver Characteristics: Implicit Double precision Dynamic memory handling SMP and MPP 2D solver / 3D solver Makes use of an automatic volume mesh generator for fluid domain Coupling with structural and thermal LS-DYNA solvers ◦ ICFD Solver Main Features: Incompressible fluid solver Thermal solver for fluids Free Surface flows Two-phase flows Turbulence models Transient or steady-state problems Non-Newtonian fluids Boussinesq model for convection Loose or strong coupling for FSI (Fluid-structure interaction) Exact boundary condition imposition for FSI problems INTRODUCTION ◦ ICFD Solver Applications (Non-exhaustive) : External aerodynamics for incompressible flows Internal aerodynamics for incompressible flows Sloshing, Slamming and Wave impacts FSI problems Conjugate heat transfer problems • Keyword family: *MESH_, the keywords starting with *MESH refer to and control the tools for the automatic volume mesh generator for the CESE and ICFD solvers. ◦ Mesh Generator Characteristics: Automatic Robust Generic Tetrahedral elements for 3D, Triangles in 2D Closed body fitted mesh (surface mesh) needs to be provided for vol- ume generation ◦ Mesh Generator Main Features: Automatic remeshing to keep acceptable mesh quality for FSI prob- lems (ICFD only) Adaptive meshing tools (ICFD only) Anisotropic boundary layer mesh Mesh element size control tools Remeshing tools for surface meshes to ensure mesh quality ◦ Mesh Generator Applications : Used by the Incompressible CFD solver (ICFD). Used by the Compressible CFD solver (CESE). Other additions to Version 7 include: • Add new parameter VNTOPT to *AIRBAG_HYBRID, that allows user more control on bag venting area calculation. • Allow heat convection between environment and CPM bag (*AIRBAG_PARTI- CLE) bag. Apply proper probability density function to part's temperature created by the particle impact. • *AIRBAG_PARTICLE and *SENSOR_SWITCH_SHELL_TO_VENT allows user to input load curve to control the venting using choking flow equation to get proper probability function for vents. Therefore, this vent will have the same vent rate as real vent hole. INTRODUCTION • Add new option NP2P in *CONTROL_CPM to control the repartition frequency of CPM particles among processors (MPP only). • Enhance *AIRBAG_PARTICLE to support a negative friction factor (FRIC or PFRIC) in particle to fabric contact. Particles are thus able to rebound at a trajec- tory closer to the fabric surface after contact. • Use heat convection coefficient HCONV and fabric thermal conductivity KP to get correct effective heat transfer coefficient for heat loss calculation in *AIRBAG_PARTICLE. If KP is not given, H will be used as effective heat trans- fer coefficient. • Extend CPM inflator orifice limit from 100 to unlimited (*AIRBAG_PARTICLE). • Support dm_in_dt and dm_out_dt output to CPM chamber database (*DATA- BASE_ABSTAT) to allow user to study mass flow rate between multiple cham- bers. • Previously, the number of ships (rigid bodies) in *BOUNDARY_MCOL, as specified by NMCOL, was limited to 2. Apparently, this was because the code had not been validated for more than 2 rigid bodies, but it is believed that it should not be a problem to remove this restriction. Consequently, this limit has been raised to 10, with the caveat that the user should verify the results for NM- COL > 2. a • Implemented structural-acoustic mapping (*BOUNDARY_- ACOUSTIC_MAPPING), for mapping transient structural nodal velocity to acoustic volume surface nodes. This is useful if the structure finite element mesh and the acoustic boundary/finite element mesh are mismatched. scheme • *CONTACT_FORMING_ONE_WAY_SURFACE_TO_SURACE_ORTHO_FRIC- TION can now be defined by part set IDs when supplemented by *DEFINE_- FRICTION_ORIENTATION. Segment sets with orientation per *DEFINE_FRIC- TION_ORIENTATION are generated automatically. • Contact force of *CONTACT_ENTITY is now available in intfor (*DATABASE_- BINARY_INTFOR). • *CONTACT_FORCE_TRANSDUCER_PENALTY will now accept node sets for both the slave and master sides, which should allow them to work correctly for eroding materials. BOTH sides should use node sets, or neither. • Added option to create a backup penalty-based contact for a tied constraint- based contact in the input (IPBACK on Card E of *CONTACT). • New option for *CONTACT_ENTITY. If variable SO is set to 2, then a con- straint-like option is used to compute the forces in the normal direction. Friction is treated in the usual way. • *CONTACT_ENTITY: allow friction coefficient to be given by a “coefficient vs time” load curve (input < 0 -> absolute value is the load curve ID). Also, if the friction coefficient bigger or equal 1.0, the node sticks with no sliding at all. INTRODUCTION • Minor tweak to the way both MPP and SMP handle nodes sliding off the ends of beams in *CONTACT_GUIDED_CABLE. • Frictional energy output in sleout (*DATABASE_SLEOUT) supported for *CON- TACT_…_MORTAR. • Tiebreak damage parameter output as “contact gap” in intfor file for *CON- OP- TACT_AUTOMATIC_SURFACE_TO_SURFACE_TIEBREAK_MORTAR, TION = 9. • Added MPP support for *CONTACT_2D_AUTOMATIC_SINGLE_SURFACE and *CONTACT_2D_AUTOMATIC_SURFACE_TO_SURFACE. • Added keyword *CONSTRAINED_MULTIPLE_GLOBAL for defining multi- node constraints for imposing periodic boundary conditions. • Enhancement for *CONSTRAINED_INTERPOLATION_SPOTWELD (SPR3): calculation of bending moment is more accurate now. • If *CONSTRAINED_NODAL_RIGID_BODY nodes are shared by several processors with mass scaling on, the added mass is not summed up across processors. This results in an instability of the NRB. (MPP only) • *ALE_REFINE has been replaced and expanded upon by the *CONTROL_RE- FINE family of commands. These commands invoke local mesh refinement of shells, solids, and ALE elements based on various criteria. • Shells or solids in a region selected for refinement (parent element) are replaced by 4 shells or 8 solids, respectively. *CONTROL_REFINE_SHELL applies to shells, *CONTROL_REFINE_SOLID applies to solids and *CONTROL_RE- FINE_ALE and *CONTROL_REFINE_ALE2D applies to ALE elements. Each keyword has up to 3 lines of input. If only the 1st card is defined, the refinement occurs during the initialization. The 2nd card defines a criterion CRITRF to automatically refine the elements during the run. If the 3rd card is defined, the refinement can be reversed based on a criterion CRITM. All commands are implemented for MPP. • *CONTROL_REFINE_MPP_DISTRIBUTION distributes the elements required by the refinement across the MPP processes. • Eliminate automatic writing of a d3plot plot state after each 3D tetrahedral remeshing operation (*CONTROL_REMESHING) to reduce volume of output. • Generate disbout output (*DATABASE_DISBOUT) for MPP and SMP binout files. • Extend *DATABASE_MASSOUT to include option to output mass information on rigid body nodes. • Added new keyword *CHANGE_OUTPUT for full deck restart to override default behavior of overwriting existing ASCII files. For small restart, this option INTRODUCTION has no effect since all ASCII output is appended to the result of previous run already. • Added new option (NEWLENGD) to 2nd field of 3rd card of *CONTROL_OUT- PUT to write more detailed legend in ASCII output files. At present, only rcforc and jntforc are implemented. • Increased default binary file size scale factor (x=) from 7 to 1024. That means the default binary file size will be 1 Gb for single version and 2 Gb for double ver- sion. • Add echo of new “max frequency of element failure summaries” flag (FRFREQ in *CONTROL_OUTPUT) to d3hsp file. • Support LSDA/binout output for new pllyout file (*DATABASE_PLLYOUT, *ELEMENT_BEAM_PULLEY) in both SMP and MPP. • Allow degenerated hexahedrons for cohesive solid elements (ELFORM = 19, 20) that evolve from an extrusion of triangular shells. The input of nodes on the element cards for such a pentahedron is given by: N1, N2, N3, N3, N4, N5, N6, N6. (pentas) • Add new option to activate drilling constraint force for shells in explicit calculations. This can be defined by parameters DRCPSID (part set) and DR- CPRM (scaling factor) on *CONTROL_SHELL. • Add SMP ASCII database “pllyout” (*DATABASE_PLLYOUT) for *ELEMENT_- BEAM_PULLEY. • *FREQUENCY_DOMAIN_ACOUSTIC_BEM: ◦ Added an option to output real part of acoustic pressure in time domain. ◦ Enabled BEM acoustic computation following implicit transient analysis. ◦ Implemented coupling between steady state dynamics and collocation acoustic BEM. ◦ Implemented Acoustic Transfer Vector (ATV) to variational indirect BEM acoustics. ◦ Enabled boundary acoustic mapping in BEM acoustics. • *FREQUENCY_DOMAIN_ACOUSTIC_FEM: ◦ Added boundary nodal velocity to binary plot file d3acs. ◦ Implemented pentahedron elements in FEM acoustics. ◦ Enabled using boundary acoustic mapping in FEM acoustics. • *FREQUENCY_DOMAIN_FRF: ◦ Updated FRF to include output in all directions (VAD2 = 4). ◦ Added treatment for FRF with base acceleration (node id can be 0). INTRODUCTION • *FREQUENCY_DOMAIN_RANDOM_VIBRATION: ◦ Updated calculation of PSD and RMS von Mises stress in random vibration environment, based on Sandia National Laboratories report, 1998. • *FREQUENCY_DOMAIN_RANDOM_VIBRATION_FATIGUE: ◦ Implemented an option to incorporate initial damage ratio in random vi- bration fatigue. • *FREQUENCY_DOMAIN_RESPONSE_SPECTRUM: ◦ Implemented double sum methods (based on Gupta-Cordero coefficient, modified Gupta-Cordero coefficient, and Rosenblueth-Elorduy coefficient). ◦ Updated calculating von Mises stress in response spectrum analysis. ◦ Implemented treatment for multi simultaneous input spectra. ◦ Improved double sum methods by reducing number of loops. • *FREQUENCY_DOMAIN_SSD: ◦ Added the option to output real and imaginary parts of frequency re- sponse to d3ssd. ◦ Added the option to output relative displacement, velocity and accelera- tion in SSD computation in the case of base acceleration. Previously only absolute values were provided. • Implemented keyword *FREQUENCY_DOMAIN_MODE_{OPTION} so that user can select the vibration modes to be used for frequency response analysis. • Implemented keyword *SET_MODE_{OPTION} so that user can define a set of vibration modes, to be used for frequency response analysis. • Implemented keyword *FREQUENCY_DOMAIN_PATH to define the path of binary databases containing mode information, used in restarting frequency domain analysis, e.g. frf, ssd, random vibration. • Compute normal component of impulse for oblique plates in *INITIAL_MINE_- IMPULSE. The feature is no longer limited to horizontal plates. • Disable license security for *INITIAL_IMPULSE_MINE. The feature is no longer restricted. • Enabled hourglass type 7 to work well with *INITIAL_FOAM_REFERENCE_- GEOMETRY so that initial hourglass energy is properly calculated and foam will spring back to the initial geometry. • Accommodate erosion of thin shells in *LOAD_BLAST_ENHANCHED. INTRODUCTION • *LOAD_VOLUME_LOSS has been changed such that after the analysis time exceeds the last point on the curve of volume change fraction versus time, the volume change is no longer enforced. • *LOAD_BODY_POROUS new option AOPT added to assign porosity values in material coordinate system. • Added *LOAD_SEGMENT_FILE. • Add new sensor definition, *SENSOR_DEFINE_ANGLE. This card traces the angle formed between two lines. • *SENSOR_DEFINE_NODE can be used to trace the magnitude of nodal values (coordinate, velocity or accleration) when VID is “0” or undefined. • Add two new parameters to *SENSOR_DEFINE_ELEMENT, scale factor and power, so that user can adjust the element-based sensor values (strain, stress, force, …). • Change history variables 10-12 in *MAT_054/*MAT_ENHANCED_COMPOS- ITE_DAMAGE (thin shells only) to represent strains in material coordinate system rather than in local element coordinate system. This is a lot more helpful for postprocessing issues. This change should not lead to different results other than due to different round-off errors. • New features and enhancements to *MAT_244/*_MAT_UHS_STEEL: ◦ Added implicit support for MAT_244. ◦ Changed the influence of the austenite grain size in Mat244 according to Li et al. ◦ Changed the start temperatures to fully follow WATT et al and Li et al. ◦ Hardness calculation is now improved when noncontinuous cooling is ap- plied i.e., tempering. ◦ Added temperature dependent Poisson ratio and advanced reaction kinet- ics. ◦ Added new advanced option to describe the thermal expansion coeffi- cients for each phase. ◦ Added option to use Curve ID or a Table ID for describing the latent heat generation during phase transormations. ◦ Added support for table definition for Youngs modulus. Now you can have one temperature dependent curve for each of the 5 phases • Added support for implicit to *MAT_188. • Added material model *MAT_273/*MAT_CDPM/*MAT_CONCRETE_DAM- AGE_PLASTIC_MODEL. This model is aimed at simulations where failure of concrete structures subjected to dynamic loadings is sought. The model is based on effective stress plasticity and has a damage model based on both plastic and elastic strain measures. Implemented for solids only but both for explicit and INTRODUCTION implicit simulations. Using an implicit solution when damage is activated may trigger a slow convergense. IMFLAG = 4 or 5 can be useful. • Added an option in *MAT_266 (*MAT_TISSUE_DISPERSED) so that the user can tailor the active contribution with a time dependent load curve instead of using the internal hardcoded option. See ACT10 in the User's Manual. • *MAT_173/*MAT_MOHR_COULOMB is available in 2D. • Enable *MAT_103 and *MAT_104 to discretize the material load curves accord- ing to the number of points specified by LCINT in *CONTROL_SOLUTION. • Implement Prony series up to 18 terms for shells using *MAT_076/*MAT_GEN- ERAL_VISCOELASTIC. • Added *DEFINE_STOCHASTIC_VARIATION and the STOCHASTIC option for *MATs 10, 15, 24, 81, 98 for shells, solids, and type 13 tets. This feature defines a stochastic variation in the yield stress and damage/failure of the aforementioned material models. • Add Moodification for *DEFINE_CONNECTION_PROPERTIES, PROPRUL = 2: thinner weld partner is first partner, PROPRUL = 3: bottom (nodes 1-2-3-4) weld partner is first partner. • Add spotweld area to debug output of *DEFINE_CONNECTION_PROPERTIES which is activated by *CONTROL_DEBUG. • Add support of *MAT_ADD_EROSION option NUMFIP < 0 for standard (non- GISSMO) failure criteria. Only for shells. • Improve implicit convergence of *MAT_ADD_EROSION damage model GISS- MO by adding damage scaling (1-D) to the tangent stiffness matrix. • Provide plastic strain rates (tension/compression, shear, biaxial) as history variables no. 16, 17, and 18 for *MAT_187. • Add new variables to user failure routine matusr_24 (activated by FAIL < 0 on *MAT_024 and other materials): integration point numbers and element id. • Add new energy based, nonlocal failure criterion for *MAT_ADD_EROSION, parameters ENGCRT (critical energy) and RADCRT (critical radius) after EP- STHIN. Total internal energy of elements within a radius RADCRT must exceed ENGCRT for erosion to occur. Intended for windshield impact. • Add new option to *MAT_054 for thin shells: Load curves for rate dependent strengths and a rate averaging flag can be defined on new optional card 9. • Add new option for *MAT_MUSCLE: Input parameter SSP < 0 can now refer to a load curve (stress vs. stretch ratio) or a table (stress vs. stretch ratio vs. normal- ized strain rate). • Expand list of variables for *MAT_USER_DEFINED_MATERIAL_MODELS by characteristic element size and element id. INTRODUCTION • Enable *MAT_USER_DEFINED_MATERIAL_MODELS tetrahedron element type 13. “umat41v_t13” show corresponding pressure calculation in the elastic case. to be used with New sample routines “umat41_t13” and • Add a new feature to *MAT_125 allowing C1 and C2 to be used in calculation of back stress. When plastic strain < 0.5%, C1 is used, otherwise C2 is used as described in Yoshida's paper. • Extend non-linear strain path (_NLP_FAILURE) in *MAT_037 to implicit. • *MAT_173/*MAT_MOHR_COULOMB now works in ALE. A new option has been added to suppress the tensile limit on hydrostatic stress recommended for ALE multi-material use. • Upgraded *MAT_172/*MAT_CONCRETE_EC2. ◦ Corrections to DEGRAD option. ◦ Concrete and reinforcement types 7 and 8 have been added to reflect changes to Eurocode 2. ◦ Extra history variables for reinforcement stress and strain are now output as zero for zero-fraction reinforcement directions. • Added RCDC model for solid *MAT_082. • Added Feng's failure model to solid *MAT_021. • Added *MAT_027 for beams. • Added *DEFINE_HAZ_PROPERTIES and *DEFINE_HAZ_TAILOR_WELDED_- BLANK for modifying material behavior near a spot weld. • Added fourth rate form to viscoplastic Johnson-Cook model (*MAT_015). • Added option to *MAT_224 to not delete the element if NUMINT = -200. • New damage initiation option 3 in multi fold damage criteria in *MAT_ADD_- EROSION. Very similar to option 2 but insensitive to pressure. • Added rotational resistance in *MAT_034/*MAT_FABRIC. Optionally the user may specify the stiffness, yield and thickness of and elastic-perfectly-plastic coated layer of a fabric that results in a rotational resistance during the simula- tion. • FLDNIPF < 0 in *MAT_190/*MAT_FLD_3-PARAMETER_BARLAT for shell elements means that failure occurs when all integration points within a relative distance of -FLDNIPF from the mid surface has reached the fld criterion. • A computational welding mechanics *MAT_270/*MAT_CWM material is available that allows for element birth based on a birth temperature as well as annealing based on an annealing temperature. The material is in addition a thermo-elasto-plastic material with kinematic hardening and temperature de- pendent properties. INTRODUCTION • Added *MAT_271/*MAT_POWDER, a material (i.e., compaction and sintering) of cemented carbides. It is divided into an elastic- plastic compaction model that is supposed to be run in a first phase, and a visco- elastic sintering model that should be run in a second phase. This model is for solid elements. for manufacturing • For IHYPER = 3 on a *MAT_USER_DEFINED_… shell material, the deformation gradient is calculated from the geometry instead of incremented by the velocity gradient. The deformation gradient is also passed to the user defined subrou- tines in the global system together with a transformation matrix between the global and material frames. This allows for freedom in how to deal with the deformation gradient and its transformations in orthotropic (layered) materials. • The Bergstrom-Boyce viscoelastic rubber model is now available in explicit and implicit analysis as *MAT_269/*MAT_BERGSTROM_BOYCE_RUBBER. The Arruda-Boyce elastic stress is augmented with a Bergstrom-Boyce viscoelastic stress corresponding to the response of a single entangled chain in a polymer gel matrix. • Added a new parameter IEVTS to *MAT_USER_DEFINED_MATERIAL_MOD- ELS (*MAT_041-050). IEVTS is optional and is used only by thick shell formula- tion 5. It points to the position of E(a) in the material constants array. Following E(a), the next 5 material constants must be E(b), E(c), v(ba), v(ca), and v(cb). This data enables thick shell formulation 5 to calculate an accurate thickness strain, otherwise the thickness strain will be based on the elastic constants pointed to by IBULK and IG. • Implemented enhancements to fabric material (*MAT_034), FORM = 14. Stress- strain curves may include a portion for fibers in compression. When un- load/reload curves with negative curve ID are input (curve stretch options), the code that finds the intersection point now extrapolates the curves at their end rather than simply printing an error message if an intersection point cannot be found before the last point in either curve. • Map 1D to 3D by beam-volume averaging the 1D data over the 3D elements (*INITIAL_ALE_MAPPING). • In a 3D to 3D mapping (*INITIAL_ALE_MAPPING), map the relative displace- ments for the penalty coupling in *CONSTRAINED_LAGRANGE_IN_SOLID. • The [name].xy files associated with *DATABASE_ALE_MAT are now created when sense switches sw1, sw2, quit, or stop are issued. • *ALE_ESSENTIAL_BOUNDARY is available in 2D. • *DATABASE_FSI is available for 2D (MPP). • *ALE_ESSENTIAL_BOUNDARY implemented to apply slip-only velocity BC along ALE mesh surface. INTRODUCTION • *CONTROL_ALE flag INIJWL = 2 option added to balance initial pressure state between ALE Soil and HE. • Include SPH element (*ELEMENT_SPH) in time step report. • Time step and internal energy of 2D axisymmetric SPH elements are calculated in a new way more consistent with the viscosity force calculation. • Only apply viscosity force to x and y components of 2D axisymmetric SPH element, not on hoop component. • MAXV in *CONTROL_SPH can be defined as a negative number to turn off velocity checking. • Improve calculation of 2D axisymmetric SPH contact force in *DEFINE_SPH_- TO_SPH_COUPLING. • Added the following material models for SPH particles: *MAT_004/*MAT_- ELASTIC_PLASTIC_THERMAL (3D only) and *MAT_106/*MAT_ELASTIC_- VISCOPLASTIC_THERMAL • Added a new parameter DFACT for *DEFINE_SPH_TO_SPH_COUPLING. DFACT invokes a viscous term to damp the coupling between two SPH parts and thereby reduce the relative velocity between the parts. • Added BOUNDARY_CONVECTION and BOUNDARY_RADIATION for explicit SPH thermal solver. • *CONTROL_REMESHING_EFG: ◦ Add eroding failed surface elements and reconstructing surface in EFG adaptivity. ◦ Add a control parameter for monotonic mesh resizing in EFG adaptivity. ◦ Add searching and correcting self-penetration for adaptive parts in 3D tet- rahedron remeshing. • Enhance 3D axisymmetric remeshing with 6-node/8-node elements • (*CONTROL_REMESHING): ◦ Use RMIN/RMAX along with SEGANG to determine element size. ◦ Remove the restriction that the reference point of computational model has to be at original point (0, 0, 0). ◦ Rewrite the searching algorithm for identifying the feature lines of cross- sections in order to provide more stable remeshing results. • Improve rigid body motion in EFG shell type 41. • Support EFG pressure smoothing in EFG solid type 42 for *MAT_ELASTIC_VIS- COPLASTIC_THERMAL. • Add visco effect for implicit EFG solid type 42. INTRODUCTION • Add new EFG solid type 43 (called Meshfree-Enriched FEM, MEFEM) for both implicit and explicit. This element formulation is able to relieve the volumetric locking for nearly-incompressible material (eg. rubber) and performs strain smoothing across elements with common faces. • EFG shell adaptivity no longer requires a special license. • Application of EFG in an implicit analysis no longer requires a special license. • Add *SENSOR_CONTROL for prescribed motion constraints in implicit. • Update *INTERFACE_LINKING_NODE in implicit to catch up with explicit, including adding scaling factors. • Add support for *DATABASE_RCFORC_MOMENT for implicit. • Enhance Iterative solvers for Implicit Mechanics. • Add, after the first implicit time step, the output of projected cpu and wall clock times. This was already in place for explicit. Also echo the termination time. • Add variable MXDMP in *CONTROL_THERMAL_SOLVER to write thermal conductance matrix and right-hand side every MXDMP time steps. • Add keyword *CONTROL_THERMAL_EIGENVALUE to calculate eigenval- ue(s) of each thermal conductance matrix. • Added thermal material model *MAT_THERMAL_ORTHOTROPIC_TD_LC. This is an orthtropic material with temperature dependent properties defined by load curves. • Changed structured file format for control card 27 (first thermal control card). Several input variables used i5 format limiting their value to 99,999. A recent large model exceeded this limit. The format was changed to i10. This change is not backward compatible. Old structured input files will no longer run unless control card 27 is changed to the new i10 format. This change does not affect the KEYWORD file. • Add thermal material *MAT_T07/*MAT_THERMAL_CWM for welding simulations, to be used in conjunction with mechanical counterpart *MAT_- 270/*MAT_CWM. • Modify decomposition costs of *MAT_181 and *MAT_183. • Introduce new timing routines and summary at termination. • Echo “MPP contact is groupable” flag to d3hsp • Bodies using *MAT_RIGID_DISCRETE were never expected to share nodes with non-rigid bodies, but this now works in MPP. • There is no longer any built-in limitation on the number of processors that may be used in MPP. INTRODUCTION • Echo contents of the MPP pfile (including keyword additions) to the d3hsp and mes0000 files. • Add new keyword *CONTROL_MPP_PFILE, which allows for insertion of text following this command to be inserted into the MPP pfile (p = pfile). • Change in MPP treatment of *CONSTRAINED_TIE-BREAK. They now share a single MPI communicator, and a single round of communication. This should improve performance for problems with large numbers of these, without affect- ing the results. • Added two input variables for *CONTROL_FORMING_ONESTEP simulation, TSCLMIN is a scale factor limiting the thickness reduction and EPSMAX defines the maximum plastic strain allowed. • Added output of strain and stress tensors for onestep solver *CONTROL_FORM- ING_ONESTEP, to allow better evaluation of formability. • Improved *CONTACT_AUTO_MOVE: before changes the termination time, and it causes problems when several tools need to be moved. Now *CONTACT_AU- TO_MOVE does not change the termination time, but changes the current time. In this way, several tools can be moved without the need to worry about the other tool's move. This is especially useful in multi-flanging and hemming simulations. • Made improvements to previously undocumented keyword *INTERFACE_- BLANKSIZE, including adding the options_INITIAL_TRIM, and_INITIAL_- ADAPTIVE. This keyword was developed for blank size development in sheet metal forming. Generally, for a single forming process, only the option_DEVEL- OPMENT is needed and inputs are an initial estimated blank shape, a formed blank shape, and a target blank shape in either mesh or boundary coordinates. Output will be the calculated/corrected initial blank shape. Initial blank mesh and formed blank mesh can be different (e.g. adaptive). For a multi-stamping process involving draw, trimming and flanging, all three options are needed. Related commands for blank size estimation are *CONTROL_FORMING_ON- ESTEP, and for trim line development, *CONTROL_FORMING_UNFLANGING. • Made improvements and added features to previously undocumented keyword *CONTROL_FORMING_UNFLANGING, this keyword unfolds flanges of a deformable blank, e.g., flanged or hemmed portions of a sheet metal part, onto a rigid tooling mesh using the implicit static solver. It is typically used in trim line mapping during a draw die development process. The roots of the flanges or hemmed edges are automatically processed based on a user input of a distance tolerance between the flanges/hemmed edges and rigid tool. It includes the ability to handle a vertical flange wall. Other keywords related to blank size development are, *CONTROL_FORMING_ONESTEP, and *INTERFACE_- BLANKSIZE_DEVELOPMENT. INTRODUCTION • Added keyword *CONTROL_FORMING_OUTPUT which allows control of d3plot output by specifying distances to tooling home. It works with automatic position of stamping tools using *CONTROL_FORMING_AUTOPOSITION_PA- RAMETER. • Added the LOCAL_SMOOTH option to *INTERFACE_COMPENSATION_NEW which features smoothing of a tool's local area mesh, which could otherwise become distorted due to, e.g., bad/coarse mesh of the original tool surface, tooling pairs (for example, flanging post and flanging steel) do not maintain a constant gap and several compensation iterations. This new option also allows for multiple regions to be smoothed. Local areas are defined by *SET_LIST_- NODE_SMOOTH. • Added output to rcforc for *DEFINE_DE_TO_SURFACE_COUPLING. • Implement traction surface for *DEFINE_DE_TO_SURFACE_COUPLING. • Add keyword *DATABASE_BINARY_DEMFOR with command line option dem = dem_int_force. This will turn on the DEM interface force file for DEM coupling option. The output frequency is controlled by the new keyword. • Add new feature *DEFINE_DE_INJECTION to allow DEM particle dropping from user defined plane. • Add new option_VOLUME to *ELEMENT_DISCRETE_SPHERE. This will allow DEM input based on per unit density and use *MAT card to get consistent material properties. • Added FORM = -4 for *ELEMENT_SHELL_NURBS_PATCH. Rotational dofs are automatically set at control points at the patch boundaries, whereas in the interior of the patch only translational dofs are present. This helps for joining multiple nurbs patches at their C0-boundaries. • Disabled FORM = 2 and 3 for *ELEMENT_SHELL_NURBS_PATCH. These formulations are experimental and not fully validated yet. • Added energy computation for isogeometric shells (*ELEMENT_SHELL_- NURBS_PATCH) to matsum. • Allow isogeometric shells (*ELEMENT_SHELL_NURBS_PATCH) to behave as rigid body (*MAT_RIGID). • Added “g” as abbreviation for gigawords in specification of memory on execution line, e.g, memory = 16g is 16 billion words. • Suppress non-printing characters in *COMMENT output. • Add command line option “pgpkey” to output the current public PGP key used by LS-DYNA. The output goes to the screen as well as a file named “lstc_ pgpkey.asc” suitable for directly importing into GPG. INTRODUCTION • When reading the NAMES file, allow a “+” anywhere on a line to indicate there will be a following line, not just at the end. This was never intended, but worked before r73972 and some customers use it that way. • Check for integer overflow when processing command line arguments and the memory value on the *KEYWORD card. • Added new capability for *INTERFACE_LINKING_NODE to scale the dis- placements of the moving interface. • Support for *KEYWORD_JOBID with internal *CASE driver. • *DAMPING_FREQUENCY_RANGE now works for implicit dynamic solutions. An error check has been added to ensure that the timestep is small enough for the damping card to work correctly. • Added new option *DAMPING_FREQUENCY_RANGE_DEFORM to damp only the deformation instead of the global motion. • Added *DEFINE_VECTOR_NODES. A vector is defined using two node IDs. • Add sense switch “prof” to output current timing profile to message (SMP) file or mes#### (MPP) files. Also, for MPP only, collect timing information from processor and output to prof.out when sense switch “prof” is detected. Capabilities added during 2013/2014 to create LS-DYNA R7.1: • Add MUTABLE option for *PARAMETER so that parameter values can be redefined later in the input deck. • Change MPP treatment of two-sided *CONTACT_FORCE_TRANSDUCER so that proper mass and moment values can be output to the rcforc file. • MPP support for non-zero birthtime for *CONTACT_SINGLE_EDGE. • Add new command line option “ldir=” for setting a local working directory. In MPP, this has the same effect as setting the “directory { local }” pfile option (and it overrides that option). For SMP, it indicates a directory where local, working files should be placed. • Add support for SMOOTH option in MPP groupable contact. • Add new keyword card *CONTROL_REQUIRE_REVISION to prevent the model from being run in old versions of LS-DYNA. • Add part set specification for dynamic relaxation with implicit using *CON- TROL_DYNAMIC_RELAXATION. This is a new feature specified with idrflg = 6 on *CONTROL_DYNAMIC_RELAXATION. This allows implicit to be used for the dynamic relaxation phase for models involving parts being modeled with SPH and/or ALE while excluding those parts from the dynamic relaxation phase. INTRODUCTION • Add new feature for implicit automatic time step control to cooperate with thermal time step control. On *CONTROL_IMPLICIT_AUTO, IAUTO = 2 is the same as IAUTO = 1 with the extension that the implicit mechanical time step is limited by the active thermal time step. • On *CONTROL_IMPLICIT_SOLUTION, add negative value of MAXREF for implicit mechanics. Nonlinear iteration will terminate after |MAXREF| itera- tions. With MAXREF < 0 convergence is declared with a warning. Simulation will continue. Positive values of MAXREF still cause failure of convergence to be declared leading to either a time step reduction or an error termination. • Add *CONTROL_IMPLICIT_MODAL_DYNAMIC keywords and features. This elevates the modal dynamic features of IMASS = 2 on *CONTROL_IMPLICIT_- DYNAMICS. It also adds additional features of damping and mode selection and stress computations. • New material model *MAT_DRY_FABRIC / MAT_214, which can be used in modeling high strength woven fabrics with transverse orthotropic behavior. • Add *ALE_COUPLING_NODAL_PENALTY, penalty-based nodal coupling with ALE. • Add type 8 *ELEMENT_SEATBELT_PRETENSIONER which takes energy-time curve, instead of pull-in or force curve. • Add type 9 *ELEMENT_SEATBELT_PRETENSIONER for energy-based buckle / anchor pretensioner. • Add *DATABASE_BINARY_FSILNK. This feature stores coupling pressure from *CONSTRAINED_LAGRANGE_IN_SOLID in a binary time history file for use in a separate model that does not include ALE. • Add *LOAD_SEGMENT_FSILNK. Use pressure loads stored in aforementioned binary time history file to load model that does not have ALE elements. • Add new keyword *DEFINE_SPH_DE_COUPLING to allow SPH particles to contact discrete element spheres (DES). • Add MOISTURE option to *MAT_076 solids. Allows moisture content to be input as a function of time. Material parameters are then scaled according to the moisture and a moisture strain is also introduced. • Add *RIGIDWALL_FORCE_TRANSDUCER to output forces from rigidwalls acting on node sets. • Add LOG_INTERPOLATION option to *MAT_024. This offers an alternate means of invoking logarithmic interpolation for strain rate effects. The other way is to input the natural log of strain rate in the table LCSS. • Add capability in *MAT_ADD_EROSION (NUMFIP < -100) to set stress to zero in each shell integration point as it reaches the failure criterion. When |NUMFIP|-100 integration points have failed, the shell is eroded. In contrast, INTRODUCTION when NUMFIP > 0, failed integration points continue to carry full load as though they were unfailed until element erosion occurs. • Add new keyword, *PARAMETER_TYPE, for use by LS-PrePost when combin- ing keyword input files. The appropriate offset is applied to each ID value defined using *PARAMETER_TYPE, according to how that ID is used. • Allow use of load curve to specify damping as a function of time in *DAMP- ING_RELATIVE. • Add a segment based (SOFT = 2) contact option to include the overlap area in the contact stiffness calculation. This is good for improving the friction calculation and possibly for implicit convergence. The option is turned on by setting FNLSCL > 0 and DNLSCL = 0. As DNLSCL = 0, the contact stiffness is not nonlinear. This new option is also useful when used with another improvement that was made to the FS = 2 friction coefficient by table lookup option in segment based contact. When the above mentioned FNLSCL > 0, option is used, the FS = 2 option is now very accurate. • Add a new RCDC damage option, *MAT_PLASTICITY_WITH_DAMAGE_OR- THO_RCDC1980 which is consistent with the WILKINS paper. It uses the principal values of stress deviators and a different expression for the A_d term. • Add a TIETYP option to *CONTACT_2D_AUTOMATIC. By default the tied contact automatically uses constraint equations when possible for 2D tied con- tact. If a conflict is detected with other constraints, or to avoid 2-way constraints, penalty type ties are used when constraints are not possible. The TIETYP option, when set to 1, causes all ties to use the penalty method. This is useful if in spite of the code's best efforts to avoid problems, there is still a conflict in the model. • Add a scale factor for scaling the frictional stiffness for contact. The parameter is FRICSF on optional card E and it's only supported for segment based (SOFT = 2) contact. This was motivated by a rubber vs. road skidding problem where the friction coefficent had static, dynamic and decay parameters defined. The growth of the frictional force was too slow so the static coulomb value could not be achieved. By scaling the frictional stiffness higher, the coulomb value could approach the static value. • Add keyword *CONTACT_2D_AUTOMATIC_FORCE_TRANSDUCER. Like the 3D force transducers, it does no contact calculation but only measures the contact forces from other contact definitions. When only a slave side is defined, the contact force on those segments is measured. Currently, two surface force transducers are not available. • Add options to *MAT_058: ◦ Load curves for rate dependent strain values (E11C, E11T, …) can be de- fined on new optional card 9. INTRODUCTION ◦ Load curves for rate dependent strengths (XC, XT, …) and a rate averaging flag can be defined on new optional card 8. ◦ Abscissa values in above curves are taken to be natural log of strain rate when the first value is negative. ◦ Add optional transverse shear damage to *MAT_058. • Add MAT_261 and MAT_262 for general use. *MAT_261 is *MAT_LAMINA- *MAT_262 is *MAT_LAMINATED_ TED_FRACTURE_DAIMLER_PINHO. FRACTURE_DAIMLER_CAMANHO. • Add pentahedra cohesive solid element types (TYPE = 21 & 22). Type = 21 is the pentahedra version of Type = 19 and Type = 22 is the pentahedra version of Type = 20. Using ESORT.gt.0 in *CONTROL_SOLID will automatically sort out the pentahedra elements (19 to 21 and 20 to 22). • Add *DEFINE_DE_BY_PART to define control parameters for DES by part ID, including damping coefficient, friction coefficient, spring constant, etc. If de- fined, it will overwrite the parameters in *CONTROL_DISCRETE_ELEMENT. • Add new feature for *MAT_030 (*MAT_SHAPE_MEMORY) as optional 3rd card. Curves or tables (strain rate dependency) can be defined to describe plastic loading and unloading behavior. • New feature for *ELEMENT_BEAM_PULLEY. Beam elements BID1 and BID2 can now both be defined as “0” (zero). In that case, adjacent beam elements are automatically detected. Therefore, the first two beam elements with nodal distance < 1.0e-6 to the pulley node (PNID) will be chosen. • Add new feature to *MAT_ADD_EROSION's damage model GISSMO. By default, damage is driven by equivalent plastic strain. Now, users can optionally define another history variable as driving quantity by setting DMGTYP. • Add volumetric plastic strain to *MAT_187 as history variable 6. • Add internal energy calculation for *ELEMENT_BEAM_PULLEY. • Add viscoplastic option to *MAT_157: new parameter VP on Card 5, Column 6. • Add new keyword *MAT_ADD_COHESIVE which is intended to make 3D material models available for cohesive elements. • Add new parameters to *MAT_CABLE_DISCRETE / *MAT_071. MXEPS (Card 2, Column 4) is equal the maximum strain at failure and MXFRC (Card 2, Col- umn 5) is equal to the maximum force at failure • Add *MAT_124 as potential weld partner material for PROPRUL = 2/3 of *DE- FINE_CONNECTION_PROPERTIES. • Add new material *MAT_TOUGHENED_ADHESIVE_POLYMER (TAPO) or *MAT_252 for epoxy-based, toughened, ductile adhesives. INTRODUCTION • Add new option to *MAT_002_ANIS: parameter IHIS on Card 4, Column 8. IHIS = 0: terms C11, C12, … from Cards 1, 2, and 3 are used. IHIS = 1: terms C11, C12, … initialized by *INITIAL_STRESS_SOLID's extra history variables. • Add new option to *MAT_102. Instead of constant activation energy Q, one can define a load curve LCQ on Card 2, Column 7: ◦ LCQ.GT.0: Q as function of plastic strain ◦ LCQ.LT.0: Q as function of temperature • Add new option to *MAT_071 (MAT_CABLE_DISCRETE_BEAM). New parameter FRACL0 (Card 2, Column 3) is fraction of initial length that should be reached over time period of TRAMP. That means the cable element length gets modified from L0 to FRACL0*L0 between t = 0 and t = TRAMP. • Add internal energy calculation for SPR models *CONSTRAINED_INTERPOLA- TION_SPOTWELD (SPR3) and *CONSTRAINED_SPR2. Their contribution was missing in energy reports like glstat. • Add new failure model OPT = 11 to *MAT_SPOTWELD/*MAT_100 for beam elements. • Add three new failure criteria for shell elements to *MAT_ADD_EROSION on optional card 4, columns 6-8: ◦ LCEPS12: load curve in-plane shear strain limit vs. element size. ◦ LCEPS13: load curve cross-thickness shear strain limit vs. element size. ◦ LCEPSMX: load curve in-plane major strain limit vs. element size. • Add new capability to *MAT_ADD_EROSION damage model GISSMO. Strain rate scaling curve LCSRS can now contain natural logarithm values of strain rates as abscissa values. This is automatically assumed when the first value is negative. • Add new parameter NHMOD to *MAT_266. The constitutive model for the isotropic part can now be chosen: ◦ NHMOD = 0: original implementation (modified Neo-Hooke) ◦ NHMOD = 1: standard Neo-Hookeon (as in umat45) • New keyword *DEFINE_TABLE_MATRIX is an alternative way of defining a table and the curves that the table references from a single unformatted text file, e.g., as saved from an Excel spreadsheet. • Change long format so that all data fields are 20 columns and each line of input can hold up to 200 columns. In this way, the number of input lines is the same for long format as for standard format. ◦ 8 variables per line in long format = 160 columns INTRODUCTION ◦ 10 variables per line in long format = 200 columns • Add a new option (SOFT = 6) in *CONTACT_FORMING_NODES_TO_SUR- FACE for blank edge and guide pin contact. • Add user-defined criteria for mesh refinement (or coarsening) in *CONTROL_- REFINE_…. • Add new contact option that currently only works for MPP SINGLE_SURFACE contact with SOFT = 0 or 1. If SRNDE (field 4 of optional card E) is a 1, then free edges of the contact definition will be rounded WITHOUT extending the seg- ments. Rather than having cylindrical caps on the ends of the segments, the “corners” of the squared off thickness are rounded over. • Add geometric contact entity type -3 “finite cylinder”. • Add irate = 2 to *CONTROL_IMPLICIT_DYNAMICS to turn off rate effects for both implicit and explicit. • Add quadratic 8-node and 6-node shells (shell formulations 23 and 24). • Add LOG_LOG_INTERPOLATION option for table defining strain rate effects in *MAT_083, *MAT_181, and *MAT_183. • Add automatic generation of null shells for quadratic shell contact (*PART_DU- PLICATE_NULL_OVERLAY). • Add beam contact forces to rcforc output (*DATABASE_RCFORC). • Add SHL4_TO_SHL8 option to *ELEMENT_SHELL to automatically convert 4- node shells to 8-node quadratic shells. • Add 3-node beam element with quadratic interpolation that is tailored for the piping industry. It includes 12 degrees of freedom, including 6 ovalization degrees of freedom, per node for a total of 36 DOF. An internal pressure can be given that can stiffen and elongate the pipe. ◦ ELFORM = 14 in *SECTION_BEAM. ◦ *ELEMENT_BEAM_ELBOW. ◦ NEIPB in *DATABASE_EXTENT_BINARY to direct output of elbow loop- stresses to d3plot. Otherwise, output goes to ASCII file elbwls.k. ◦ Supported by a subset of material models including mats 3, 4, 6, 153, 195. • Add discrete element option DE to *DATABASE_TRACER. ◦ Includes variable RADIUS. average result of all RADIUS > 0: Reports the average result of all DE particles in a spher- ical volume having radius = RADIUS and centered at the tracer. RADIUS < 0: Reports result of the closest particle to the tracer. INTRODUCTION ◦ If a tracer node NID is given, then the tracer moves with this node. The node must belong to a DES. • Add new options *PART_COMPOSITE_LONG and *ELEMENT_SHELL_COM- POSITE_LONG. In contrast to “COMPOSITE”, one integration point is defined per card. This is done to allow for more informations, e.g. new variable “ply id”. • Add support of *MAT_ADD_EROSION option NUMFIP < 0 for standard (non- GISSMO) failure criteria. Only for shells. • Add viscoplastic behavior to *MAT_157, i.e., parameter LCSS can now refer to a table with strain rate dependent yield curves. • Add singular finite element with midside nodes for 2D plane strain fracture analysis (ELFORM = 55 in *SECTION_SHELL). This is an 8-noded element and can induce a singular displacement field by moving mid-side nodes to quarter locations. • If HCONV < 0 in *AIRBAG_PARTICLE, |HCONV| is a curve of heat convection coefficient vs. time. • Add new option DECOMPOSITION for *AIRBAG_PARTICLE -- MPP only.This will automatically invoke the recommended decomposition commands, *CON- TROL_MPP_DECOMPOSITION_BAGREF (if applicable) and *CONTROL_- MPP_DECOMPOSITION_ARRANGE_PARTS, for the bag. • Add new blockage option for vents in *AIRBAG_PARTICLE: ◦ blockage considered .eq.0: no .eq.1: yes .eq.2: yes, exclude external vents .eq.3: yes, exclude internal vents .eq.4: yes, exclude all vents • Add option in *CONTROL_CPM to consider CPM in the time step size calcula- tion. • When using *AIRBAG_PARTICLE with IAIR = 2, user should keep mole / particle similar between inflator gas and initial air particles to ensure the correct elastic collision. If different by more than 10%, code will issue warning message and provide the suggested initial air particle number. • Enable *DEFINE_CURVE_FUNCTION for *SECTION_POINT_SOURCE_MIX- TURE and *SECTION_POINT_SOURCE. • Make *BOUNDARY_PRESCRIBED_MOTION_SET compatible with *CON- TROL_REFINE INTRODUCTION • Change *BOUNDARY_ACOUSTIC_COUPLING_MISMATCH to rank order opposing acoustic faces and structural segments by proximity, thereby accelerat- ing the preprocessing stage, enhancing reliability and allowing some liberaliza- tion of the search parameters. • Implement hemispherical geometry for particle blast (*DEFINE_PBLAST_- GEOMETRY). • Add explosive type for *PARTICLE_BLAST. • For particle-based blast *PARTICLE_BLAST: ◦ Include random distribution of initial air molecules ◦ Modify algorithm to account for the non-thermally-equilibrated state of high velocity gas. • Improve particle contact method for particle-based blast loading *PARTICLE_- BLAST. • *CONTACT now works for parts refined using *CONTROL_REFINE_SOLID or *CONTROL_REFINE_SHELL. • Improve calculation of shell element contact segment thicknesses, particularly at material boundaries. • MPP: Add output to rcforc file for *CONTACT_AUTOMATIC_TIEBREAK to record the # of nodes tied, and the total tied area. • MPP: Add calculation of “contact gap” for master side of FORMING contact. • MPP: Add support for table-based friction (FS = 2.0) to groupable contact. • Implement splitting-pinball contact, Belytschko & Yeh (1992, 1993). This new contact option is invoked by setting SOFT = 2, SBOPT = 3 and DEPTH = 45. A penetration check method based on LS-PrePost version 4.0 is implemented for the new bilinear-patch-based contact, SOFT = 2, DEPTH = 45 & Q2TRI = 0. The new method provides more accurate intersection information when Q2TRI = 0. • Add support for birth time for *CONTACT_2D_AUTOMATIC_TIED. • Improve the segment based single surface contact search for thick segment pairs that are too close together. The code was not working well with triangluar segments. This change affects models with shell segments that have thickness greater than about 2/3 of the segment length. • Enable segment based quad splitting options to work when shell sets or segment sets are used to define the surface that will be split. This is really a bug fix because there was no check to prevent this and the result was writing past the allocated memory for segment connectivites. • Allow *CONSTRAINED_INTERPOLATION to use node set to define the independent nodes. INTRODUCTION • Add a length unit to the tolerance used for the checking of noncoincident nodes in *CONSTRAINED_JOINTs excluding spherical joints. The old tolerance was 1.e-3. The new tolerance is 1.e-4 times the distance between nodes 1 and 3. The error messages were changed to warnings since this change might otherwise cause existing models to stop running. • Add d3hsp output for *CONSTRAINED_INTERPOLATION_SPOTWELD (SPR3) and *CONSTRAINED_SPR2. Can be deactivated by setting NPOPT = 1 on *CONTROL_OUTPUT. • Support NFAIL1 and NFAIL4 of *CONTROL_SHELL in coupled thermal- mechanical analysis, i.e. erode distorted elements instead of error termination. • PTSCL on *CONTROL_CONTACT can be used to scale contact force exerted on shell formulations 25, 26, 27 as well as shell formulations 2, 16 (IDOF = 3). • Use SEGANG in *CONTROL_REMESHING to define positive critical angle (unit is radian) to preserve feature lines in 3D tetrahedral remeshing (ADPOPT = 2 in *PART). • For 3D solid adaptive remeshing including ADPOPT = 2 and ADPOPT = 3 (*PART), the old mesh will be used automatically if the remesher fails generating a new mesh. • Add option INTPERR on *CONTROL_SHELL (Optional Card 3, Column 8). By default, warning messages INI+143/144/145 are written in case of non-matching number of integration points between *INITIAL_STRESS_SHELL and *SEC- TION_SHELL. Now with INTPERR = 1, LS-DYNA can terminate with an error. • Add variable D3TRACE on *CONTROL_ADAPTIVE: The user can now force a plot state to d3plot just before and just after an adaptive step. This option is necessary for tracing particles across adaptive steps using LS-PrePost. • By putting MINFO = 1 on *CONTROL_OUTPUT, penetration info is written to message files for mortar contact., see also *CONTACT_…. Good for debugging implicit models, not available for explicit. • Change the default scale factor for binary file sizes back to 70. This value can be changed using “x=” on the execution line. In version R7.0, the default value of x is 4096, and that sometimes leads to difficulty in postprocessing owing to the large size of the d3plot file(s). • Enable *CONTROL_OUTPUT flag, EOCS, which wasn't having any effect on the shells output to elout file. • *DATABASE_FSI_SENSOR: Create sensors at solid faces in 3D and at shell sides in 2D. • *DATABASE_PROFILE: Implement the option DIR = 4 to plot data with curvilinear distributions and the flag UPDLOC to update the profile positions. • In *CONTROL_SHELL, add options for deletion of shells based on: INTRODUCTION ◦ diagonal stretch ratio (STRETCH) ◦ w-mode amplitude in degrees (W-MODE) • New element formulation ELFORM = 45 in *SECTION_SOLID: Tied Meshfree- enriched FEM (MEFEM). This element is based on the 4-noded MEFEM element (ELFORM = 43, *SECTION_SOLID). Combined with *CONSTRAINED_TIED_- NODES_FAILURE, *SET_NODE_LIST and cohesive model, this element can be used to model dynamic multiple-crack propagation along the element bounda- ries. • New high order tetrahedron CPE3D10 based on Cosserat Point theory can be invoked by specifying element formulation ELFORM = 16 and combining this with hourglass formulation IHQ = 10. See *SECTION_SOLID and *HOUR- GLASS. • Add database D3ACS for collocation acoustic BEM (*FREQUENCY_DOMAIN_- ACOUSTIC_BEM) to show the surface pressure and normal velocities. • Implement biased spacing for output frequencies for random vibration (*FRE- QUENCY_DOMAIN_RANDOM_VIBRATION). • Add frequency domain nodal or element velocity output for acoustic BEM (*FREQUENCY_DOMAIN_ACOUSTIC_BEM). • Implement boundary acoustic mapping to acoustic BEM in MPP (*BOUND- ARY_ACOUSTIC_MAPPING). This is enabled only for segment sets at present. • Implement panel contribution analysis capability to Rayleigh method (*FRE- QUENCY_DOMAIN_ACOUSTIC_BEM_PANEL_CONTRIBUTION). • Implement a scheme to map velocity boundary condition from dense BEM mesh to coarse mesh to speed up the computation (*FREQUENCY_DOMAIN_- ACOUSTIC_BEM). • Add user node ID for acoustic field points in D3ATV (*FREQUENCY_DO- MAIN_ACOUSTIC_BEM). Now D3ATV is given for multiple field points, and multiple frequencies. • Add database D3ATV for acoustic transfer vector binary plot (*FREQUENCY_- *DATABASE_FREQUENCY_BINARY_- DOMAIN_ACOUSTIC_BEM_ATV, D3ATV). • Implement acoustic panel contribution analysis to collocation BEM and dual collocation BEM (*FREQUENCY_DOMAIN_ACOUSTIC_BEM). • Enable *FREQUENCY_DOMAIN_MODE in response spectrum analysis (*FRE- QUENCY_DOMAIN_RESPONSE_SPECTRUM). • Implement an option to read in user-specified nodal velocity history data for running BEM acoustics (*FREQUENCY_DOMAIN_ACOUSTIC_BEM). INTRODUCTION • Extend Kirchhoff acoustic method to MPP (*FREQUENCY_DOMAIN_- ACOUSTIC_BEM). • Extend response spectrum analysis to multiple load spectra cases (*FREQUEN- CY_DOMAIN_RESPONSE_SPECTRUM). • Add BAGVENTPOP for *SENSOR_CONTROL. This allows user more flexibilty controlling the pop-up of the venting hole of *AIRBAG_HYBRID and *AIRBAG_WANG_NEFSKE • Add command *SENSOR_DEFINE_FUNCTION. Up to 15 *DEFINE_SENSORs can be referenced in defining a mathematical operation. • LAYER of *SENSOR_DEFINE_ELEMENT can now be an integer “I” represent- ing the Ith integration point at which the stress/strain of the shell or tshell ele- ment will be monitored. • Add control of *LOAD_MOVING_PRESSURE by using *SENSOR_CONTROL. • Add thick shells to the ETYPE option list of *SENSOR_DEFINE_ELEMENT. • Add *CONTROL_MPP_MATERIAL_MODEL_DRIVER in order to enable the Material Model Driver for MPP (1 core). • Add table input of thermal expansion coefficient for *MAT_270. Supports temperature-dependent curves arranged according to maximum temperature. • Add table input of heat capacity for *MAT_T07. Supports temperature depend- ent curves arranged according to maximum temperature. • Add two more kinematic hardening terms for *MAT_DAMAGE_3/MAT_153, c2 & gamma2. • Add materials *MAT_CONCRETE_DAMAGE_REL3/*MAT_072R3 and *MAT_- CSCM_CONCRETE/*MAT_159 to Interactive Material Model Driver. • Enable *MAT_JOHNSON_COOK/*MAT_015 for shell elements to work with coupled structural / thermal analysis. • Allow *MAT_SOIL_AND_FOAM/*MAT_005 to use positive or negative abscissa values forload curve input of volumetric strains. • Add *MAT_ACOUSTIC elform = 8 support for pyramid element case using 5-pt integration. • Add support to *MAT_219 (*MAT_CODAM2) for negative AOPT values which point to coordinate system ID's. • Modify *MAT_224 so it uses the temperatures from the thermal solution for a coupled thermal-mechanical problem. • Add alternative solution method (Brent) for *MAT_015 and *MAT_157 in case standard iteration fails to converge. INTRODUCTION • Add shell element IDs as additional output to messag file for *MAT_036's warning “plasticity algorithm did not converge”. • For *MAT_USER_DEFINED_MATERIAL_MODELS, the subroutines crvval and tabval can be called with negative curve / table id which will extract values from the user input version of the curve or table instead of the internally converted “100-point” curve / table. • In the damage initiation and evolution criteria of *MAT_ADD_EROSION (invoked by IDAM < 0), add the option Q1 < 0 for DETYP = 0. Here, |Q1| is the table ID defining the ufp (plastic displacement at failure) as a function of triaxial- ity and damage value, i.e., ufp = ufp(eta, D), as opposed to being constant which is the default. • In *MAT_RHT, ONEMPA = -6 generates parameters in g, cm, and 𝜇S and ONEMPA = -7 generates parameters in g, mm, and mS • In *MAT_SIMPLIFIED_RUBBER/FOAM, STOL > 0 invokes a stability analysis and warning messages are issued if an unstable stretch point is found within a logarithmic strain level of 100%. • Implement *DATABASE_ALE to write time history data (volume fractions, stresses, …) for a set of ALE elements. Not to be confused with *DATABASE_- ALE_MAT. • Implement *DELETE_PART in small restarts for ALE2D parts. • Add conversion of frictional contact energy into heat when doing a coupled thermal-mechanical problem for SPH (variable FRCENG in *CONTROL_CON- TACT). This option applys to all 3D contact types supported by SPH particles. • For keyword *DEFINE_ADAPTIVE_SOLID_TO_SPH, add support of explicit SPH thermal solver for the newly generated SPH particles which were converted from solid elements. The temperatures of those newly generated SPH particles are mapped from corresponding solid elements. • Implement DE to surface tied contact *DEFINE_DE_TO_SURFACE_TIED. The implementation includes bending and torsion. • Implement keyword *DEFINE_DE_HBOND to define heterogeneous bond for discrete element spheres (DES). DES (*ELEMENT_DISCRETE_SPHERE) with different material models can be bonded. • Implement keyword *INTERFACE_DE_BOND to define multiple failure models for various bonds within one part or between different parts through the key- word *DEFINE_DE_HBOND. • Implement *DEFINE_DE_TO_BEAM_COUPLING for coupling of discrete element spheres to beam elements. INTRODUCTION • Add variable MAXGAP in *DEFINE_DE_BOND to give user control of distance used in judging whether to bond two DES together or not, based on their initial separation. • Add IAT = -3 in *CONTROL_REMESHING_EFG, which uses FEM remapping scheme in EFG adaptivity. Compared to IAT = -2, -1, 1, 2, IAT = -3 is faster and more robust but less accurate. • Add control flag MM in *CONTROL_REMESHING_EFG to turn on/off monotonic mesh resizing for EFG 3D general remeshing (ADPOPT = 2 in *PART). • *CONTROL_IMPLICIT_BUCKLING - Extend Implicit Buckling Feature to allow for Implicit problems using Inertia Relief. This involves adding the Power Method as a solution technology for buckling eigenvalue problems. Using the power method as an option for buckling problems that are not using inertia relief has been added as well. • Extend Implicit Buckling to allow for Intermittent extraction by using negative values of NMODE on *CONTROL_IMPLICIT_BUCKLING similar to using negative values of NEIG on *CONTROL_IMPLICIT_EIGENVALUE. • Extend implicit-explicit switching specified on *CONTROL_DYNAMIC_RELAX- ATION to allow explicit simulation for the dynamic relaxation phase and implic- it for the transient phase. • New implementation for extracting resultant forces due to joints for implicit mechanics. • New implementation of extracting resultant forces due to prescribed motion for implicit mechanics. • Add support for IGAP > 2 in implicit, segment based (SOFT = 2) contact. • Add constraint-based, thermal nodal coupling for *CONSTRAINED_LA- GRANGE_IN_SOLID. HMIN < 0 turns it on. • Add FRCENG = 2 on CONTROL_CONTACT keyword. ◦ if FRCENG = 1, convert contact frictional energy to heat. ◦ if FRCENG = 2, do not convert contact frictional energy to heat. • Add effect of thermal time scaling (TSF in *CONTROL_THERMAL_SOLVER) to 2D contact. • Add new pfile decomposition region option: partsets. Takes a list of part sets (*SET_PART) from the keyword input and uses them to define a region, e.g., region { partsets 102 215 sy 1000 } This example would take partsets, scale y by 1000, and decompose them and distribute them to all processors. • Reduce MPP memory usage on clusters. • Add MPP support for *ELEMENT_SOURCE_SINK. INTRODUCTION • Add new pfile options: ◦ decomp { d2r_as_rigid } ◦ decomp { d2ra_as_rigid } which cause materials appearing in “*DEFORMABLE_TO_RIGID” and “*DE- FORMABLE_TO_RIGID_AUTOMATIC” to have their computational costs set as if they were rigid materials during the decomposition. • Add option ISRCOUT to *INCLUDE_STAMPED_PART to dump out the transformed source/stamp mesh. • *CONTROL_FORMING_OUTPUT: Allow NTIMES to be zero; support birth and death time; support scale factor in curve definition. • Add a new option (INTFOR) to *CONTROL_FORMING_OUTPUT to control the output frequency of the INTFOR database. • Add new features (instant and progressive lancing) in *ELEMENT_LANCING for sheet metal lancing simulation. • Add a new keyword: *CONTROL_FORMING_INITIAL_THICKNESS. • Add a new option for springback compensation: *INCLUDE_COMPENSA- TION_ORIGINAL_TOOLS. • Add a new keyword: *INTERFACE_COMPENSATION_NEW_PART_- CHANGE. • Add a new keyword (*DEFINE_CURVE_BOX_ADAPTIVITY) to provide better control of mesh refinement along two sides of the curve. • Isogeometric analysis: contact is available in MPP. • Normalize tangent vectors for local coordinate system for the rotation free isogeometric shells. • Add support for dumping shell internal energy density for isogeometric shells (*ELEMENT_SHELL_NURBS_PATCH) via interpolation shells. • Add support for dumping of strain tensor (STRFLG.eq.1) for isogeometric shells (*ELEMENT_SHELL_NURBS_PATCH) via interpolation shells. • Add H-field, magnetization and relative permeability to d3plot output. • *ICFD_INITIAL: Add a reference pressure (pressurization pressure) for when no pressure is imposed on the boundaries. • Add the initialization of all nodes at once by setting PID = 0. • Add the non-inertial reference frame implementation defined by the keyword *ICFD_DEFINE_NONINERTIAL. • Add several new state variables to LSO. Please refer to the LSO manual to see how to print out the list of supported variables. INTRODUCTION • Add support for FSI with thick shells. • 2D shells are now supported for FSI in MPP. In the past only beams could be used in MPP and beams and shells could be used in SMP. • The keyword ICFD_CONTROL_FSI has a new field to control the sensitivity of the algorithm to find the solid boundaries used in FSI calculations. • The 2D mesh now generates semi-structured meshes near the boundaries. • Add heat flux boundary condition using ICFD_BOUNDARY_FLUX_TEMP. • Add divergence-free and Space Correlated Synthetic Turbulence Inlet Boundary Condition for LES (Smirnov et al.) using *ICFD_BOUNDARY_PRESCRIBED_- VEL. • *ICFD_BOUNDARY_PRESCRIBED_VEL: Add inflow velocities using the wall normal and a velocity magnitude using the 3rd field VAD. • Add the activation of synthetic turbulence using the 3rd field VAD. • Add the option to control the re-meshing frequency in both keywords: see *ICFD_CONTROL_ADAPT_SIZE and *ICFD_CONTROL_ADAPT. • *ICFD_CONTROL_TURB_SYNTHESIS: control parameters for the synthetic turbulence inflow. • *ICFD_BOUNDARY_PRESCRIBED_MOVEMESH: Allows the mesh to slide on the boundaries following the cartesian axis. • Add a PART_SET option for *CESE_BOUNDARY_…_PART cards. • Bring in more 2D mesh support, both from the PFEM mesher and a user input 2D mesh (via *ELEMENT_SOLID with 0 for the last 4 of 8 nodes). • Enable the 2D ball-vertex mesh motion solver for the 2D CESE solver. • Add new input cards: ◦ *CESE_BOUNDARY_CYCLIC_SET ◦ *CESE_BOUNDARY_CYCLIC_PART • Add code for 2D CESE sliding boundary conditions. • Add support in CESE FSI for 2D shells in MPP. • Add support for CESE FSI with thick shells. • Add 2D & 2D-axisymmetric cases in the CESE-FSI solver (including both immersed boundary method & moving mesh method) . • Add the CSP reduced chemistry model with 0D, 2D, and 3D combustion. The 2D and 3D combustion cases couple with the CESE compressible flow solver. • Add the G-scheme reduced chemistry model only for 0D combustion. • Add two different reduced chemistry models. INTRODUCTION ◦ The Computational Singular Perturbation (CSP) reduced model is imple- mented with existing compressible CESE solver. The CSP is now working on 0-dimensional onstant volume and pressure combustion, 2-D, and 3-D combustion problems. ◦ The new reduced chemistry model, G-scheme, is implemented, but cur- rently works only 0-dimensional problems such as constant combustors. • Jobid can now be changed in a restart by including “jobid=“ on the restart execution line. Previously, the jobid stored in d3dump could not be overwritten. • Part labels (PID) can be up to 8 characters in standard format; 20 characters in long format. • Labels for sections (SID), materials (MID), equations of state (EOSID), hourglass IDs (HGID), and thermal materials (TMID) can be up to 10 characters in standard format; 20 characters in long format. • Create bg_switch and kill_by_pid for SMP. Both files will be removed at the termination of the run. • Increase the overall length of command line to 1000 characters and length of each command line option to 50 characters. • Increase MPP search distance for tied contacts to include slave and master thicknesses. • For *CONTACT_AUTOMATIC_…_MORTAR, the mortar contact now supports contact with the lateral surface of beam elements. • On *CONTACT_..._MORTAR, IGAP.GT.1 stiffens the mortar contact for large penetrations. The mortar contact has a maximum penetration depth DMAX that depends on geometry and input parameters; if penetration is larger than this value the contact is released. To prevent this release, which is unwanted, the user may put IGAP.GT.1 which stiffens the behavior for penetrations larger than 0.5*DMAX without changing the behavior for small penetrations. This should hopefully not be as detrimental to convergence as increasing the overall contact stiffness. • For initialization by prescribed geometry in dynamic relaxation (IDRFLG = 2, *CONTROL_DYNAMIC_RELAXATION), add an option where displacements are not imposed linearly but rather according to a polar coordinate system. This option was added to accommodate large rotations. • The flag RBSMS on *CONTROL_RIGID is now active for regular and selective mass scaling to consistently treat interfaces between rigid and deformable bodies • Remove static linking for l2a as many systems do not have the required static libraries. • Add IELOUT in *CONTROL_REFINE to handle how child element data is handled in elout (*DATABASE_HISTORY_SOLID and *DATABASE_HISTO- INTRODUCTION RY_SHELL). Child element data are stored if IELOUT = 1 or if refinement is set to occur only during initialization. • Include eroded hourglass energy in hourglass energy in glstat file to be con- sistent with KE & IE calculations so that the total energy = kinetic energy + internal energy + hourglass energy + rigidwall energy. • Remove *DATABASE_BINARY_XTFILE since it is obsolete. • When using *PART_AVERAGED for truss elements (beam formulation 3), calculate the time step based on the total length of the combined macro-element instead of the individual lengths of each element. • Enable writing of midside nodes to d3plot or 6- and 8-node quadratic shell elements. • Write complete history variables to dynain file for 2D solids using *MAT_NULL and equation-of-state. • Shell formulations 25, 26, and 27 are now fully supported in writing to dynain file (*INTERFACE_SPRINGBACK_LSDYNA). • Shell formulations 23 (quad) and 24 (triangle) can now be mixed in a single part. When ESORT = 1 in *CONTROL_SHELL, triangular shells assigned by *SEC- TION_SHELL to be type 23 will automatically be changed to type 24. • Enable hyperelastic materials (those that use Green's strain) to be used with thick shell form 5. Previously, use of these materials (2, 7, 21, 23, 27, 30, 31, 38, 40, 112, 128, 168, and 189) with thick shell 5 has been an input error. • Update acoustic BEM to allow using *DEFINE_CURVE to define the output frequencies (*FREQUENCY_DOMAIN_ACOUSTIC_BEM). • When using *CONTROL_SPOTWELD_BEAM, convert *DATABASE_HISTO- RY_BEAM to *DATABASE_CROSS_SECTION and *INITIAL_AXIAL_FORCE_- BEAM to *INITIAL_STRESS_CROSS_SECTION for the spotweld beams that are converted to hex spotwelds. • Improve output of *INITIAL_STRESS_BEAM data to dynain via *INTERFACE_- SPRINGBACK_LSDYNA. Now, large format can be chosen, history variables are written, and local axes vectors are included. • Update *MAT_214 (*MAT_DRY_FABRIC) to allow fibers to rotate independent- ly. • Enable regularization curve LCREGD of *MAT_ADD_EROSION to be used with FLD criterion, i.e. load curve LCFLD. Ordinate values (major strain) will be scaled with the regularization factor. • Modify *MAT_ADD_EROSION parameter EPSTHIN: ◦ EPSTHIN > 0: individual thinning for each IP from z-strain (as before). ◦ EPSTHIN < 0: averaged thinning strain from element thickness (new). INTRODUCTION • Enable regularization curve LCREGD of *MAT_ADD_EROSION to be used with standard (non-GISSMO) failure criteria. Users can now define a failure criterion plus IDAM = 0 plus LCREGD = scaling factor vs. element size to get a regular- ized failure criterion. • *MAT_ADD_EROSION: equivalent von Mises stress SIGVM can now be a function of strain rate by specifying a negative load curve ID. • *SECTION_ALE1D and *SECTION_ALE2D now work on multiple processors (SMP and MPP). • *CONSTRAINED_LAGRANGE_IN_SOLD ctype 4/5 now converts friction energy to heat. Note it only works for ALE elform 12. Capabilities added September 2013 – January 2015 to create LS-DYNA R8.0: See release notes (published separately) for further details. • Add RDT option for *AIRBAG_SHELL_REFERENCE_GEOMETRY. • LCIDM and LCIDT of *AIRBAG_HYDRID can now be defined through *DE- FINE_CURVE_FUNCTION. • New variable RGBRTH in *MAT_FABRIC to input part-dependent activation time for airbag reference geometry. • Negative PID of *AIRBAG_INTERACTION considers the blockage of partition area due to contact. • Enhancements to *AIRBAG_PARTICLE: ◦ New blockage (IBLOCK) option for vents. ◦ External work done by inflator gas to the structure is reported to glstat. ◦ Enhance segment orientation checking of CPM bag and chambers. ◦ Allow user to excluded some parts surface for initial air particles. ◦ Support compressing seal vent which acts like flap vent. ◦ Support Anagonye and Wang porosity equation through *MAT_FABRIC. ◦ Add keyword option _MOLEFRACTION. • Add_ID keyword option *AIRBAG_REFERENCE_GEOMETRY and *AIRBAG_SHELL_REFERENCE which includes optional input of variables for scaling the reference geometry. to • Enable *DEFINE_CURVE_FUNCTION for *AIRBAG_SIMPLE_AIRBAG_MOD- EL. • Calculate heat convection (HCONV) between environment and airbag in consistent fashion when TSW is used to switch from a particle airbag to a control volume. INTRODUCTION • For *AIRBAG_PARTICLE, add ENH_V = 2 option for vent hole such that two- way flow can occur, i.e., flow with or against the pressure gradient. • *BOUNDARY_ALE_MAPPING: add the following mappings: 1D to 2D, 2D to 2D, 3D to 3D. • *SET_POROUS_ALE: new keyword to define the properties of an ALE porous media by an element set. The porous forces are computed by *LOAD_BODY_- POROUS. • *ALE_FSI_SWITCH_MMG: applies also now to 2D. • *ALE_SWITCH_MMG: new keyword to switch multi-material groups based on criteria defined by the user with *DEFINE_FUNCTION. • *CONTROL_ALE: Allow PREF (reference pressure) to be defined by materials. • Implement *ALE_COUPLING_NODAL_DRAG to model the drag force coupling between discrete element spheres or SPH particles and ALE fluids. • Implement *ALE_COUPLING_RIGID_BODY as an efficient alternative for constraint type coupling between ALE fluids and a Lagrangian rigid body. • Error terminate if *BOUNDARY_SPC_NODE_BIRTH_DEATH is applied to a node that belongs to a rigid body. • Modify *BOUNDARY_PRESCRIBED_ORIENTATION_VECTOR to accommo- date bodies which undergo no changes in orientation. • Add a new keyword *BOUNDARY_SPC_SYMMETRY_PLANE. • Solid part or solid part set is now allowed for *PARTICLE_BLAST. • Add ambient pressure boundary condition flag BC_P for *PARTICLE_BLAST. • New command *DEFINE_PBLAST_GEOMETRY allows the high explosive domain for*PARTICLE_BLAST to be defined by various geometric shapes. • Allow multiple *PARTICLE_BLAST definitions. • Add *DATABASE_PBSTAT to output particle blast statistics. • Output the initial volume and initial mass of HE particles and air particles for *PARTICLE_BLAST to d3hsp. • Add the command *CESE_BOUNDARY_BLAST_LOAD to allow a blast described by the *LOAD_BLAST_ENHANCED command to be used as a boundary condition in CESE. • Modify the FSI interface reflective boundary condition pressure treatment in some calculations for the moving mesh and immersed boundary solvers. • Change the CESE derivatives calculation method to use the current values of flow variables. INTRODUCTION • Add two new MAT commands for CESE solver, *CESE_MAT_000 and *CESE_- MAT_002. • Add a non-inertial reference frame solver for fluid and FSI problems using the moving-mesh method. • For the moving mesh CESE solver, replace the all-to-all communication for conjugate heat and FSI quantities with a sparse communication mechanism. • Add structural element erosion capability to the immersed boundary method CESE FSI solver (serial capability only). • Add 2D cyclic boundary conditions capability. • Add a NaN detection capability for the CESE solver. • Switch all CESE boundary conditions that use a mesh surface part to define the boundary to use the character string "MSURF" instead of "PART" in the option portion of the keyword name. • Add missing temperature interpolation in time for imposing solid temperatures as a boundary condition in the CESE solver. • Optimize the IDW-based mesh motion for the CESE moving mesh solver. • Treat the input mesh as 3D by default for the CESE solver. • All of the chemistry features mentioned below are coupled only to the CESE compressible flow solver when 2D or 3D calculations are involved. • Chemical source Jacobians have been added. • Introduce *CHEMISTRY_CONTROL_PYROTECHNIC and *CHEMISTRY_PRO- PELLANT_PROPERTIES for airbag applications. In conjuction with these com- mands, basic airbag inflator models are implemented. • The pyrotechnic inflator model using NaN3/Fe2O3 propellant is newly implemented. To connect with the existing ALE airbag solver, two load curves, mass flow rate and temperature, are saved in "inflator_outfile" as a function of time. This model computes three sub-regions: combustion chamber, gas plenum, and discharge tank. Each region can be initialized with different *CHEMISTRY_- COMPOSITION models, which means that user can compute Propellant+Gas hybrid mode. • The following 0-dimensional combustion problems have been improved: constant volume, constant pressure, and CSP. • For iso-combustion. temperature and species mass fractions as a function of time are displayed on screen and saved in "isocom.csv" to plot with LS-PrePost. • Another chemical ODE integration method has been implemented. • The output file of the pyrotechnic inflator is updated so that this file can be read from ALE solver for an airbag simulation. INTRODUCTION • 2-D and 3-D TNT gaseous blast explosives, categorized as TBX (thermobaric explosives), are implemented for the Euler equation systems (CESE-only). Also, 3-D TNT blast + aluminum combustion for serial problems is now implemented. • Implement a mix modeling method for use with CESE solvers. • Modify *CHEMISTRY-related keyword commands to allow multiple chemistry models in the same problem. • Add command *CHEMISTRY_MODEL which identifies the files that define a Chemkin chemistry model. • Modify the following commands such that the files related to the chemistry model have been removed. These commands are only used to select the type of chemistry solver: ◦ *CHEMISTRY_CONTROL_CSP ◦ *CHEMISTRY_CONTROL_FULL ◦ *CHEMISTRY_CONTROL_1D • Modify *CHEMISTRY_DET_INITIATION where the files related to the chemis- try model have been removed, and the Model ID used is inferred through a reference to a chemistry composition ID. • Modify *CHEMISTRY_COMPOSITION and *CESE_CHEMISTRY_D3PLOT to add model ID. • Add *CONTACT_TIED_SHELL_EDGE_TO_SOLID for transferring moments from shells into solids. • Add frictional energy calculation for beams in *CONTACT_AUTOMATIC_GEN- ERAL. • Enhance ERODING contacts for MPP. The new algorithm uses a completely different approach to determining the contact surface. The old algorithm started from scratch when identifying the exterior of the parts in contact. The new algorithm is smarter about knowing what has been exposed based on what is eroded, and is faster. • Force EROSOP = 1 for all ERODING type contacts, with a warning to the user if they had input it as 0. • Add error check in case of a contact definition with an empty node set being given for the slave side. • Modify output of ncforc (*DATABASE_NCFORC) in order to support output in a local coordinate system. • For ERODING contacts, reduce memory allocated for segments so each interior segment is only allocated once. • Add keyword *DEFINE_CONTACT_EXCLUSION (MPP only) to allow for nodes tied in some contacts to be ignored in certain other contacts. INTRODUCTION • Rewrite meshing of *CONTACT_ENTITY to use dynamic memory, which removes the previous limit of 100 meshed contact entities. There is now no limit. • Remove undocumented release condition for MPP’s *CONTACT_AUTOMAT- IC_TIEBREAK, options 5 and greater. • Add new experimental "square edge" option to select SOFT = 0,1 contacts. This new option applies only to AUTOMATIC_SINGLE_SURFACE and the segment- to-segment treatment of AUTOMATIC_GENERAL, and is invoked by setting SRNDE = 2 on *CONTACT's Optional Card E. This new option does not apply to SOFT = 2; SOFT = 2 square edge option is set using SHLEDG in *CONTROL_- CONTACT. • BT and DT in *CONTACT can be set to define more than one pair of birthtime/death-time for the contact by pointing to a curve or table. These pairs can be unique for the dynamic relaxation phase and the normal phase of the simulation. • Add EDGEONLY option to *CONTACT_AUTOMATIC_GENERAL to exclude node-to-segment contact and consider only edge-to-edge and beam-to-beam contact. • VDC defines the coefficient of restituion when variable CORTYP is defined. *CON- Available TACT_AUTOMATIC_SURFACE_TO_SURFACE, and *CONTACT_AUTOMAT- IC_SINGLE_SURFACE; SOFT = 0 or 1 only. *CONTACT_AUTOMATIC_NODES_TO_SURFACE, for • Enhancements for *CONTACT_AUTOMATIC_GENERAL: ◦ Add beam to beam contact option CPARM8 in *PART_CONTACT (MPP only). ◦ Add option whereby beam generated on exterior shell edge will be shifted into the shell by half the shell thickness. In this way, the shell-edge-to- shell-edge contact starts right at the shell edge and not at an extension of the shell edge . • Implement *CONTROL_CONTACT PENOPT = 3 option to *CONTACT_AUTO- *CONTACT_ERODING_NODES_TO_- MATIC_NODES_TO_SURFACE and SURFACE for SMP. • Update segment based (SOFT = 2) contact to improve accuracy at points away from the origin. The final calculations are now done with nodal and segment locations that have been shifted towards the origin so that coordinate values are small. • Enable user defined friction (*USER_INTERFACE_FRICTION; subroutine usrfrc) for MPP contact SOFT = 4. INTRODUCTION • Unify automatic tiebreak messages for damage start and final failure. SMP and MPP should now give the same output to d3hsp and messag. This affects *CONTACT_AUTOMATIC_...TIEBREAK, OPTIONs 6, 7, 8, 9, 10, and 11. • *CONTACT_ADD_WEAR: Associates wear calculations to a forming contact interface whose quantities can be posted in the intfor database file. Adaptivity is supported. • *CONTACT_..._MORTAR: ◦ Detailed warning outputs activated for mortar contact, also clarifies echoed data in d3hsp. ◦ Contact thickness made consistent with other contacts in terms of priority between ISTUPD on CONTROL_SHELL, SST on CONTACT and OPTT on PART_CONTACT. ◦ Efficency improvement of bucket sort in mortar contact allowing for signif- icant speedup in large scale contact simulations. • *CONTACT_..._MORTAR, *DEFINE_FRICTION, *PART_CONTACT: ◦ Mortar contact supports FS = -1.0, meaning that frictional coefficients are taken from *PART_CONTACT parameters. ◦ Mortar contact supports FS.EQ.-2 meaning that friction is taken from *DE- FINE_FRICTION. • *CONTACT_AUTOMATIC_SINGLE_SURFACE_MORTAR: IG- NORE.LT.0 for single surface mortar contact will ignore penetrations of seg- ments that belong to the same part. Using • Friction factors are now a function of temperature for *CONTACT_..._THER- MAL_FRICTION. • *SET_POROUS_LAGRANGIAN: new keyword to define the porosity of Lagrangian elements in an element set. The porous forces are computed by *CONSTRAINED_LAGRANGE_IN_SOLID ctype = 11 or 12. • *CONSTRAINED_LAGRANGE_IN_SOLID: CTYPE = 12 is now also available in 2D. • Add helix angle option for *CONSTRAINED_JOINT_GEARS. • Change keyword from *CONSTRAINED_BEARING to *ELEMENT_BEARING. • Enhance explicit to use the implicit inertia relief constraints. This allows implicit-explicit switching for such problems. • Add new input options to *CONTROL_IMPLICIT_INERTIA_RELIEF. ◦ user specified number of nodes ◦ user specified list of modes to constrain out. INTRODUCTION • Implement *CONSTRAINED_BEAM_IN_SOLID. This feature is basically an overhauled constraint couping between beams and Lagrangian solids that in- cludes features that make it more attractive in some cases than *CON- STRAINED_LAGRANGE_IN_SOLID, for example, in modeling coupling of rebar in concrete. • Allow *CONSTRAINED_INTERPOLATION to use node set to define the independent nodes. • Add new feature MODEL.GE.10 to *CONSTRAINED_INTERPOLATION_- SPOTWELD (SPR3). This allows parameters STIFF, ALPHA1, RN, RS, and BE- TA to be defined as *DEFINE_FUNCTIONs of thicknesses and maximum engineering yield stresses of connected sheets. • Add failure reports for *CONSTRAINED_SPR2. • Add more d3hsp output for *CONSTRAINED_INTERPOLATION_SPOTWELD and *CONSTRAINED_SPR2. Can be deactivated by setting NPOPT = 1 on *CONTROL_OUTPUT. • Add option to *CONSTRAINED_JOINT: Relative penalty stiffness can now be defined as function of time when RPS < 0 refers to a load curve. Works for SPHERICAL, REVOLUTE, CYLINDRICAL in explixit analyses. • Variable MODEL invokes new SPR4 option in *CONSTRAINED_INTERPOLA- TION_SPOTWELD. • *CONSTRAINED_JOINT_GEARS: Gear joint now supports bevel gears and similar types, i.e., the contact point does not necessarily have to be on the axis between the gear centers. • *CONSTRAINED_MULTIPLE_GLOBAL: Support multiple constraints defined on the extra DOFs of user-defined elements. • Make the *CONTROL_SHELL PSNFAIL option work with the W-MODE deletion criterion for shells. • New subcycling scheme activated for *CONTROL_SUBCYCLE and *CON- TROL_SUBCYCLE_MASS_SCALED_PART. By default the ratio between the largest and smallest time step is now 16 and the external forces are evaluated every time step. The old scheme had a hard wired ratio of 8. The ratios can be optionally changed by *CONTROL_SUBCYCLE_K_L where K is the maximum ratio between time steps for internal forces and L is likewise the ratio for external forces. • *DATABASE_PROFILE: ◦ output kinetic and internal energy profiles, ◦ output volume fraction profiles, ◦ add a parameter MMG to specify the ALE group for which element data can be output. INTRODUCTION • *DATABASE_ALE_MAT: can now use *DEFINE_BOX to compute the material energies, volumes and masses for elements inside boxes (instead of the whole mesh). • *DATABASE_TRACER_GENERATE: new keyword to create ALE tracer particles along iso-surfaces. • *DATABASE_FSI: add option to output moments created by FSI forces about each node in a node set. These moments about nodes are reported in dbfsi. • Add *DATABASE_BEARING to write brngout data pertaining to *ELEMENT_- BEARINGs. • Include eroded hourglass energy in hourglass energy in glstat file to be con- sistent with KE & IE calculations so that the total energy = kinetic energy + internal energy + hourglass energy + rigidwall energy. • Add support for new database pbstat (*DATABASE_PBSTAT) for *PARTICLE_- BLAST. ◦ internal energy and translational energy of air and detonation products ◦ force/pressure of air and detonation products for each part • *DATABASE_EXTENT_INTFOR: New parameter NWEAR on optional card governs the output of wear depth to the intfor database. • Using CMPFLG = -1 in *DATABASE_EXTENT_BINARY will work just as CMPFLG = 1, except that for *MAT_FABRIC (form 14 and form -14) and *MAT_- FABRIC_MAP the local strains and stresses will be engineering quantities in- stead of Green-Lagrange strain and 2nd Piola-Kirchhoff stress. • For some materials and elements, thermal and plastic strain tensors can be output to d3plot database, see STRFLG in *DATABASE_EXTENT_BINARY. • Add option for output of detailed (or long) warning/error messages to d3msg. See MSGFLG in *CONTROL_OUTPUT. Only a few "long" versions of warn- ings/errors at this time but that list is expected to grow. • Add two new options for rigid body data compression in d3plot; see DCOMP in *DATABASE_EXTENT_BINARY. • Add option to write revised legend to jntforc, secforc, rcforc, deforc and nodout files via input flag NEWLEG in *CONTROL_OUTPUT. This helps to avoid confusion over unassigned IDs and duplicated IDs. • If any input data is encrypted and dynain is requested, the code issues an error message and stops the job. • Solid part or solid part set is now allowed for *DEFINE_DE_TO_SURFACE_- COUPLING. • Implement *DELETE_PART for Discrete Element Sphere. INTRODUCTION • The unit of contact angle changed from radian to degree for *CONTROL_DIS- CRETE_ELEMENT. • Implement Archard's wear law to *DEFINE_DE_TO_SURFACE_COUPLING for discrete element spheres. Wear factor is output to DEM binout database. • Add damping energy and frictional energy of discrete elements to "damping energy" and "sliding interface energy" terms in glstat. • Introduce a small perturbation to the initial position of newly generated discrete elements for *DEFINE_DE_INJECTION. This allows a more random spatial distribution of the generated particles. • *INTERFACE_DE_HBOND replaces *INTERFACE_DE_BOND. Used to define the failure models for bonds linking various discrete element (DE) parts within one heterogeneous bond definition (*DEFINE_DE_HBOND). • *DEFINE_ADAPTIVE_SOLID_TO_DES: Embed and/or transform failed solid elements to DES (*ELEMENT_DISCRETE_SPHERE) particles. The DES particles inherit the material properties of the solid elements. All DES-based features are available through this transformation, including the bond models and contact algorithms. This command is essentially to DES what *DEFINE_ADAPTIVE_- SOLID_TO_SPH is to SPH particles. • Add EM orthotropic materials where the electric conductivity is a 3x3 tensor, see new card, *EM_MAT_003. • Add new keyword family, *EM_DATABASE_... which triggers the output of EM quantites and variables. All EM related ASCII outputs now start with em_***. Keywords are : ◦ EM_DATABASE_CIRCUIT ◦ EM_DATABASE_CIRCUIT0D ◦ EM_DATABASE_ELOUT ◦ EM_DATABASE_GLOBALENERGY ◦ EM_DATABASE_NODOUT ◦ EM_DATABASE_PARTDATA ◦ EM_DATABASE_POINTOUT ◦ EM_DATABASE_ROGO ◦ EM_DATABASE_TIMESTEP • Add capability to plot magnetic field lines in and around the conductors at given times, see *EM_DATABASE_FIELDLINE. ASCII output files are generated (lspp_fieldLine_xx) and are readable by LSPP in order to plot the field lines. In the future, LSPP will be capable of directly generating the field lines. • Add EM quantities in *DEFINE_CURVE_FUNCTION: ◦ EM_ELHIST for element history (at element center). ◦ EM_NDHIST for node history. INTRODUCTION ◦ EM_PAHIST for part history (integrated over the part). • Add *EM_EOS_TABULATED2 where a load curve defines the electrical conductivity vs time. • Introduce capability to use the EM solver on (thin) shells: An underlying solid mesh (hexes and prisms) is built where the EM is solved and the EM fields are then collapsed onto the corresponding shell. The EM mat for shells is defined in *EM_MAT_004. This works for EM solvers 1, 2 and 3 and the EM contact is available for shells. • Add different contact options in the *EM_CONTACT card. • Add new methods to calculate electric contact resistance between two conduc- tors for Resistive Spot Welding applications (RSW). See *EM_CONTACT_RE- SISTANCE. • Add Joule Heating in the contact resistance (*EM_CONTACT_RESISTANCE). The Joule heating is evenly spread between the elements adjacent to the faces in contact. • Add new circuit types 21 and 22 allowing users to put in their own periodic curve shape when using the inductive heating solver. This is useful in cases where the current is not a perfect sinusoidal. • Provide default values for NCYCLEBEM and NCYCLEFEM (=5000) and set default value of NUMLS to 100 in *EM_CIRCUIT. • Add two additional formulations, FORM = 3 and 4, to *PART_MODES. • Add 20-node solid element, ELFORM = 23 in *SECTION_SOLID. • Add H8TOH20 option to *ELEMENT_SOLID to convert 8-node to 20-node solids. • Add option SOLSIG to *CONTROL_OUTPUT which will permit stresses and other history variables for multi-integration point solids to be extrapolated to nodes. These extrapolated nodal values replace the integration point values normally stored in d3plot. NINTSLD must be set to 8 in *DATABASE_EX- TENT_BINARY when a nonzero SOLSIG is specified. Supported solid formula- tions are solid elements are: -1, -2, 2, 3, 4, 18, 16, 17, 23. • Activate contact thickness input from *PART_CONTACT for solids. • Made many enhancements for *PART_MODES for robustness and MPP implementation. • Add new cohesive shell element (elform = 29) for edge-to-edge connectivity between shells. This element type takes bending into account and supports MPP and implicit solvers. • Error terminate with message, STR+1296, if same node is defined multiple times in *ELEMENT_MASS_MATRIX. INTRODUCTION • Add support for negative MAXINT option in *DATABASE_EXTENT_BINARY for thick shell elements. • *ELEMENT_TSHELL: Add "BETA" as option for *ELEMENT_TSHELL to provide an orthotropic material angle for the element. • Add Rayleigh damping (*DAMPING_PART_STIFFNESS) for triangular shell element types 3 and 17. • Add new keyword *ELEMENT_BEAM_SOURCE. Purpose: Define a nodal source for beam elements. This feature is implemented for truss beam elements (ELFORM = 3) with material *MAT_001 and for discrete beam elements (ELFORM = 6) with material *MAT_071. • Add new option to *DEFINE_ELEMENT_DEATH. New variable IDGRP defines a group id for simultaneous deletion of elements. • Convert cohesive solid type 20 and 22 to incremental formulation to properly handle large rotations. Also use consistent mass. • Add Smoothed Particle Galerkin (SPG) method for solid analysis (ELFORM = 47) and corresponding keyword option *SECTION_SOLID_SPG. SPG is a true particle method in Galerkin formulation that is suitable for severe deformation problems and damage analysis. • Enhance *ELEMENT_LANCING by supporting *PARAMETER, *PARAME- TER_EXPRESSION. • Add a new feature, *CONTROL_FORMING_TRIMMING, for 2D and 3D trimming of a 3-layer, sandwich laminate blank via *DEFINE_CURVE_TRIM. • Add 3D normal trimming of solid elements via *DEFINE_CURVE_TRIM_3D. • Add new features for solid elements 2D trimming *DEFINE_CURVE_TRIM_- NEW: ◦ Allow support of arbitrary trimming vector (previously only global z di- rection was allowed). ◦ Improve trimming algorithm for speed up. ◦ Allow trimming curves to project to either the top or bottom surface. • Add a new AUTO_CONSTRAINT option to *CONTROL_FORMING_ONESTEP which is convenient for blank nesting. • Add new features to *CONTROL_FORMING_SCRAP_FALL. Previously the user was required to define the trimmed blank properly. Now the blank is trimmed by the cutting edge of the trim steel, which is defined by a node set and a moving vector. • Enhance *CONTROL_FORMING_SCRAP_FALL: Allow the node set (NDSET) on the trim steel edge to be defined in any order. • Improve *CONTROL_FORMING_ONESTEP: INTRODUCTION ◦ Reposition the initial part before unfolding, using the center element nor- mal. ◦ Add a message showing that the initial unfolding is in process. • Add 2D trimming for solid elements *DEFINE_CURVE_TRIM_NEW, support *DEFINE_TRIM_SEED_POINT_COORDINATES. • Add *CONTROL_FORMING_AUTOCHECK to detect and fix flaws in the mesh for the rigid body that models the tooling. • Add new features to *CONTROL_FORMING_UNFLANGING: ◦ The incoming flange mesh will be automatically checked for mesh quality and bad elements fixed. ◦ Allow thickness offset of deformable flange to use the blank thickness from user's input. ◦ Allow definition any node ID in the outer boundary of the flange, to speed up the search when holes are present in the part. ◦ Add a new parameter CHARLEN to limit the search region. ◦ Allow holes to exist in the flange regions. ◦ Output a suggested flange part after unflanging simulation, with the failed elements deleted from the unflanged part. ◦ Automatically define a node set and constraints for the flange boundary nodes through the user definition of three nodes. ◦ Add output of forming thickness, effective strain and trim curves after un- flanging simulation. • Add a new keyword *CONTROL_FORMING_TRIM to replace *ELEMENT_- TRIM. • Add a new keyword: *CONTROL_FORMING_UNFLANGING_OUTPUT: Failed elements are removed to come up with the trim curves. • Add new features to *INTERFACE_BLANKSIZE_DEVELOPMENT including allowing for trimming between initial and final blank. • Enhance *CONTROL_FORMING_OUTPUT for controlling the number of states. • Add *CONTROL_FORMING_TRIM_MERGE to close a user specified (gap) value in the trim curves, so each trim curve will form a closed loop, which is required for a successful trimming. • Add *CONTROL_FORMING_MAXID to set a maximum node ID and element ID for the incoming dynain file (typically the blank) in the current simulation. • Enhance *FREQUENCY_DOMAIN_ACOUSTIC_BEM: ◦ Update the boundary condition definition for BEM acoustics so that im- pedance and other user defined boundary conditions can be combined with time domain velocity boundary condition. INTRODUCTION ◦ Implement Burton-Miller BEM to MPP. ◦ Implement impedance boundary condition to Burton-Miller BEM. ◦ Implement half space option (*FREQUENCY_DOMAIN_ACOUSTIC_- BEM_HALF_SPACE) to variational indirect BEM. ◦ Implement half space option to acoustic scattering problems. ◦ Extend acoustic ATV computation to elements, in addition to nodes. ◦ Support element based ATV output in d3atv. ◦ Add an option (_MATV) to run modal acoustic transfer vector. Implement MATV to MPP. ◦ Implement running BEM Acoustics based on modal ATV (SSD excitation only). • *FREQUENCY_DOMAIN_ACOUSTIC_FEM: Enable running FEM acoustics based on restarting SSD (*FREQUENCY_DOMAIN_SSD). • Add *FREQUENCY_DOMAIN_ACOUSTIC_INCIDENT_WAVE to define the incident waves for acoustic scattering problems. To be used with *FREQUEN- CY_DOMAIN_ACOUSTIC_BEM. • Add *FREQUENCY_DOMAIN_ACOUSTIC_SOUND_SPEED to define frequen- cy dependent complex sound speed, which can be used in BEM acoustics. By using complex sound speed, the damping in the acoustic system can be consid- ered. To be used with *FREQUENCY_DOMAIN_ACOUSTIC_BEM. • *FREQUENCY_DOMAIN_FRF: Add mode dependent rayleigh damping to frf and ssd (DMPMAS and DMPSTF). • *FREQUENCY_DOMAIN_RESPONSE_SPECTRUM: ◦ Add output of nodout_spcm and elout_spcm, to get nodal results and ele- ment results at user specified nodes and elements. ◦ Add von Mises stress computation. • *FREQUENCY_DOMAIN_RANDOM_VIBRATION: Add semi-log, and linear- linear interpolation on PSD curves (parameter LDFLAG). • *FREQUENCY_DOMAIN_SSD: ◦ Add strain computation. ◦ Add parameter LC3 to define the duration of excitation for each frequency. ◦ Implement fatigue analysis option (_FATIGUE) based on ssd (sine sweep). ◦ Add option to use *DAMPING_PART_MASS and *DAMPING_PART_- STIFFNESS in SSD (DMPFLG = 1). • Add *MAT_ADD_FATIGUE to define material's SN fatigue curve for applica- tion in vibration fatigue and SSD fatigue analysis. • Add *FREQUENCY_DOMAIN_ACCELERATION_UNIT to facilitate the acceleration unit conversion. INTRODUCTION • The icfd_mstats.dat file now outputs the ten worst quality element locations (ICFD solver). • Add option in *ICFD_CONTROL_OUTPUT allowing terminal output to be written to messag file. • Add keyword *ICFD_CONTROL_OUTPUT_SUBDOM to output only part of the domain. Available for vtk, dx and gmv formats. • Add new keyword family, *ICFD_DATABASE_... which triggers the output of ICFD variables. All ICFD related output files now start with icfd_***. • Add new keyword family *ICFD_SOLVER_TOL_... which allows the user to control tolerances and iteration number for the fractional step solve, the mesh movement solve, and the heat equation solve. • Curves in *ICFD_BOUNDARY_PRESCRIBED_VEL each provide a scaling factor vs. x,y, or z coordinate, respectively. These scaling factors are applied to the velocity boundary condition. • Enable free-slip condition for FSI walls (ICFD solver). • Add new variable IDC to *ICFD_CONTROL_FSI that allows the modification of the scaling parameter that multiplies the mesh size to detect contact. • Add automatic squeezing to the ICFD elements of the boundary layer when there are two very close surfaces with poor (coarse) mesh resolution. • Add the initialization for all nodes using *ICFD_INITIAL with PID = 0. • Add a curve (LCIDSF in *ICFD_CONTROL_TIME) that scales the CFL number as a function of time. • Add a Heaviside function that allows the solution of simple multiphase problems (ICFD). • Add the computation of the heat convection coefficient (ICFD). • Add MPP support for y+ and shear for output (ICFD). • Add uniformity index (ICFD). • Add *ICFD_CONTROL_TAVERAGE to control the restarting time for compu- ting the time average values. • Implement the XMl format for vtk. See *ICFD_CONTROL_OUTPUT. • Improve temperature stabilization for thermal problems (ICFD). • Add the Generalized Flow Through Porous Media model monolithically coupled to the incompressible Navier-Stokes model. See keyword *ICFD_MAT for the new options. • Add the Anisotropic version of the Generalized Flow in Porous Media. See *ICFD_MAT for details. INTRODUCTION • Add the capability to define the porous properties using the Pressure-Velocity (P-V) experimental curves. See *ICFD_MAT. • Compute drag forces around anisotropic/isotropic porous domains (ICFD). • Extend implicit debug checking when LPRINT = 3 on *CONTROL_IMPLICIT_- SOLVER. • Add option for implicit dynamic relaxation so that only a subset of parts is active during the dynamic relaxation phase. • Extend implicit time step control via IAUTO < 0 in *CONTROL_IMPLICIT_AU- TO to linear analysis. • Add self piercing rivet capability to implicit (*CONSTRAINED_SPR2, *CON- STRAINED_INTERPOLATION_SPOTWELD). • Add MTXDMP in *CONTROL_IMPLICIT_SOLVER to dump the damping matrix from implicit mechanics. • Improve stress and strain computation induced by mode shapes. See MSTRES in *CONTROL_IMPLICIT_EIGENVALUE. • Add variable MSTRSCL to *CONTROL_IMPLICIT_EIGENVALUE for user control of geometry scaling for the stress computation. • Make SMP and MPP treatment of autospc constraints consistent. See AUTOSPC on *CONTROL_IMPLICIT_SOLVER. • Enhance output for *ELEMENT_DIRECT_MATRIX_INPUT (superelements) to describe how they are attached to the LS-DYNA model. • Enhance superelement computation (*CONTROL_IMPLICIT_MODES or *CON- TROL_IMPLICIT_STATIC_CONDENSATION): ◦ The computation of the inertia matrix in the presense of rigid bodies is cor- rect. ◦ Adjust superelement computation to accept initial velocities. ◦ Add null beams for the visualization of superelements. • Enhance implicit to allow the use of *CONSTRAINED_RIVET in conjunction with axisymmetric shell element problems. • Add output of performance statistics for the MPP implicit eigensolver to mes0000. • Add Stress computation to modal dynamics (*CONTROL_IMPLICIT_MODAL_- DYNAMIC). • Allow unsymmetric terms to the assembled stiffness matrix from some implicit features. INTRODUCTION • Enhance implicit-explicit switching (IMFLAG < 0 in *CONTROL_IMPLICIT_- GENERAL) so that curve |IMFLAG| can be defined using *DEFINE_CURVE_- FUNCTION. • Upgrade the implicit implementation of rack and pinion and screw joints so the joint is driven by relative motion of the assembly instead of absolute motion. • Add *CONTACT_1D to implicit mechanics. • *CONTROL_IMPLICIT_ROTATIONAL_DYNAMICS Rotordynamics using the implicit time integrator. is added to study • *MAT_SEATBELT is supported for implicit by introducing bending stiffness. • *INITIAL_LAG_MAPPING added to initialize a 3D Lagrangian mesh from the last cycle of a 2D Lagrangian simulation. • *ELEMENT_SHELL_NURBS_PATCH: ◦ Add support for dumping of strain tensor and shell internal energy densi- ty for isogeometric shells via interpolation shells. ◦ Add conventional mass-scaling for isogeometric shells. • *LOAD_BODY_POROUS: applies also now to 1D and 2D problems. • Add *LOAD_SEGMENT_CONTACT_MASK, which currently works in MPP only. This feature masks the pressure from a *LOAD_SEGMENT_SET when the pressure segments are in contact with another material. • Curve LCID of *LOAD_NODE can be defined by *DEFINE_CURVE_FUNC- TION. • *USER_LOADING: pass more data to user-defined loading subroutine loadud including nodal moment, nodal rotational displacement and velocity, and nodal translational mass and rotational inertia. • Add load curves for dynamic relaxation for *LOAD_THERMAL_VARIABLE. • *LOAD_SEGMENT_NONUNIFORM, *LOAD_SEGMENT_SET_NONUNI- FORM: By specifying a negative load curve ID the applied load becomes a follower force, i.e., the direction of the load is constant with respect to a local coordinate system that rotates with the segment. • Make several enhancements to *MAT_172. • *MAT_HYPERELASTIC_RUBBER (*MAT_077_H) has new thermal option for material properties. • Add *MAT_ORTHOTROPIC_PHASE_CHANGE, *MAT_ELASTIC_PHASE_- CHANGE, and • *MAT_MOONEY-RIVLIN_PHASE_CHANGE whereby elements change phase as they cross a plane in space. INTRODUCTION • Add P1DOFF to 2D seatbelt material, *MAT_SEATBELT_2D, to specify a part ID offset for the internally created 1D seatbelt elements. • All load curves for *MAT_067 can be defined via *DEFINE_FUNCTION. • Enhance *MAT_CWM: ◦ Add support for shell elements. ◦ Add support for hardening curves. Yield stress can be supplied as table depending on plastic strain and temperature. • Check diagonal elements of C-matrix of *MAT_002/MAT_{OPTION}TROPIC_ ELASTIC and error terminate with message, STR+1306, if any are negative. • Add a keyword option called MIDFAIL for *MAT_024, (MAT_PIECEWISE_LIN- EAR_PLASTICITY). When MIDFAIL appears in the keyword, failure by plastic strain will only be checked at the mid-plane. If the mid-plane fails, then the element fails. If there are an even number of integration points through the thickness, then the two points closest to the middle will check for failure and the element fails when both layers fail. • Enable solid and solid assembly spot welds (*MAT_SPOTWELD) to use the NF parameter for force filtering. • Add the shear angle in degrees as the first history variable for shell material *MAT_214 (DRY_FABRIC). • Expand from 2 to 5 the number of additional cards that can be used for the user defined weld failure, OPT = 12 or OPT = 22 on *MAT_SPOTWELD. Now a total of 46 user variables are possible. • Add a solid spot weld material option in *MAT_SPOTWELD to treat the stress state as uniaxial. This option is available for solid assemblies also. • Add *MAT_FABRIC form 24 which is a modified version of form 14. The main improvement is that the Poisson's effects work correctly with the nonlinear curves for fiber stress. Also, the output of stress and strain to d3plot are engi- neering stress and strain instead of 2nd PK stress and Green's strain. Added an option to input curves in engineering stress and strain rather than 2nd PK stress vs. Green's strain. To use this, set DATYP = -2 on *DEFINE_CURVE. • Increase maximum number of plies from 8 to 24 in a sublaminate with *MAT_- CODAM2. • Add *MAT_THERMAL_CHEMICAL_REACTION to model a material undergo- ing a chemical reaction such as an epoxy used in manufacturing composite materials. • *MAT_058: ◦ Add option to use nonlinear (elastic) stress-strain curves instead of con- stant stiffnesses (EA, EB, GAB). INTRODUCTION ◦ Add option to use strain-rate dependent nonlinear (elastic) stress-strain curves instead of constant stiffnesses (EA, EB, GAB). ◦ Add option to define proper poisson ratios PRCA and PRCB (also added in *MAT_158). • Add option to use yield curve or table in *MAT_100 (*MAT_SPOTWELD) for solid elements. • Add *MAT_157 for solid elements. This includes an optional variable IHIS that invokes *INITIAL_STRESS_SOLID to initialize material properties on an ele- ment-by-element basis. This was developed to allow a user to map/initialize anisotropic material properties from an injection molding simulation. • *MAT_157 (shells): ◦ Add anisotropic scale factor for plastic strain rate (VP = 1 only). ◦ Improve local stress projection for VP = 1. ◦ Add optional variable IHIS, similar to that described for solids above. • Add strain rate dependence to *MAT_103 for solids via a table (isotropic hardening only). • *MAT_136 (*MAT_CORUS_VEGTER): Implemented an alternative, implicit plasticity algorithm (define N.lt.0) for enhanced stability. • *MAT_244 (*MAT_UHS_STEEL): ◦ In plasticity with non-linear hardening, temperature effects and strain rate effects are now dealt with the same way they are implemented in *MAT_- 106. In particular, strain rate now refers to the plastic strain rate. ◦ Allow for the definition of start temperatures for each phase change, for cooling and heating. ◦ Account for elastic transformation strains, given as a curve wrt tempera- ture. ◦ Add feature to *MAT_244 for welding simulations. Similar to *MAT_270, material can be initialized in a quiet (ghost) state and activated at a birth temperature. • Furthermore, annealing is accounted for. • - Modify formula for Pearlite phase kinetics based on Kirkaldy and Venugoplan (1983). • • *MAT_249 (*MAT_REINFORCED_THERMOPLASTIC): Implement new material formulation for shells, which is based on additive split of stress tensor. INTRODUCTION ◦ For the thermoplastic matrix, a thermo-elasto-plastic material is imple- load temperature dependence is defined by mented,where curves/tables in the input file. the ◦ Includes hyperelastic fiber contribution. ◦ For any integration point, up to three different fiber directions can be de- fined. Their (non-linear) response to elongation and shear deformations can also be defined with load curves. ◦ Includes input parameters for anisotropic transverse shear stiffness. • *MAT_T07 (*MAT_THERMAL_CWM): Add HBIRTH and TBIRTH which are specific heat and thermal conductivity, resp., used for time t < TISTART. • One additional parameter (exponent GAMMA) for B-K law of *MAT_138. • MAT_187: Speed-up of load curve lookup for curves with many points. • Add new option "MAGNESIUM" to *MAT_233. Differences between tension and compression are included. • Add enhanced damage model with crack closure effects to *MAT_104. • Some improvements for *MAT_075 (BILKHU/DUBOIS_FOAM): Volumetric strain rate can now be averaged over NCYCLE cycles, original input curve LCRATE is instead of a rediscretized curve, and averaged strain rate is stored as history variable #3. • Add new history variables to *MAT_123: A mixed failure indicator as history variable #10 and triaxiality as #11. • Decrease memory requirements for *MAT_ADD_EROSION by 50%. • Add *MAT_098 for tetrahedral solid type 13. • Add new history variable #8 to *MAT_157 for shell elements: "Anisotropic equivalent plastic strain". • Add tangent stiffness to *MAT_224 for implicit analyses with solid and shell elements. • Put internal enery on "plastic strain" location for *MAT_027 solids. • Add new option *MAT_224: BETA .LT. 0: strain rate dependent amount given by load curve ID = -BETA • Add new flag to switch off all MAT_ADD_EROSION definitions globally. • This will be the 1st parameter "MAEOFF" on new keyword *CONTROL_MAT. • Add option to define a load curve for isotropic hardening in *MAT_135. • *MAT_CDPM is reimplemented by its original developers (Peter Grassl and Dimitros Xenos at University of Glasgow) for enhanced robustness. A new parameter EFC is introduced governing damage in compression and the bilinear law is exchanged for an exponential one. INTRODUCTION • *MAT_3-PARAMETER_BARLAT: HR = 7 is complemented with biaxial/shear hardening curves. • *MAT_FABRIC_MAP: ◦ A stress map material for detailed stress response in fabrics, stress can be prescribed through tables PXX and PYY corresponding to functions of bi- axial strain states. ◦ A compaction effect due to packing of yarns in compression is obtained by specifying BULKC (bulk modulus) and JACC (critical jacobian for the on- set of compaction effect). This results ib increasing pressure that resists membrane elements from collapsing and/or inverting. ◦ Strain rate effects can be obtained by specifying FXX and FYY which in ef- fect scales the stress based on engineering strain rate. A smoothing effect is applied by using a time window DT. ◦ A hysteresis option TH is implemented for stability, given in fraction dis- sipated energy during a cycle. Can also depend on the strain state through a table. • *MAT_GENERAL_HYPERELASTIC_RUBBER, *MAT_OGDEN_RUBBER: By specifying TBHYS.LT.0 a more intuitive interpolation of the damage vs. devia- toric strain energy is obtained. It requires however that the damage and strain energy axes are swapped. • *MAT_SIMPLIFIED_RUBBER: For AVGOPT.LT.0 the absolute value represents a time window over which the strain rates are averaged. This is for suppressing extensive noise used for evaluating stress from tables. • *MAT_FABRIC: The bending stiffness contribution in material 34, ECOAT/SCOAT/TCOAT, is now supported in implicit calculations. • Add *MAT_122_3D which is an extension of *MAT_122 to solid elements. This material model combines orthotropic elastic behavior with Hill’s 1948 aniso- tropic plasticity theory and its applicability is primarily to composite materials. • MPP groupable tied contact: Output messages about initial node movement due to projection like non-groupable routines do. • MPP tied contact initialization: ◦ Change a tolerance in groupable tied contact bucketsort to match the non- groupable code, and fix the slave node thickness used for beam nodes dur- ing initial search in non-groupable contact to match groupable contact. ◦ Update the slave node from beam thickness calculation for type 9,11, and 12 beams. • For MPP, set a "last known location" flag to give some indication of where the processors were if an error termination happens. Each writes a message to their INTRODUCTION own message file. Look for a line that says "When error termination was trig- gered, this processor was". • MPP BEAMS_TO_SURFACE contact: Remove "beam" node mass from the penalty stiffness calculation when soft = 1 is used, which matches SMP behavior. • Make sure the pfile.log file gets created in case of termination due to *CON- TROL_STRUCTURED_TERM. • Add two new decomposition region-related pfile options "nproc" and "%proc" so that any given decomposition region can be assigned to some subset of all the processors. nproc takes a single argument, which is a specific number of proces- sors. %proc takes a single argument, which is a percentage of processors to use. The old options "lump" and "distribute" are still available and are mapped to the new options thusly: ◦ lump => "nproc 1" ◦ distribute => "%proc 100.0" • Tweak MPP beam-to-beam contact routine for better handling of parallel beams. • MPP: Add support for new solid and shell cost routines, invoked with the pfile option "decomp { newcost }". Will be expanded to include beams, thick shells, etc. in the future. • MPP contact: add support for IGAP > 2 added to the SINGLE_SURFACE, AU- TOMATIC_GENERAL, and *_TO_SURFACE contacts. • Improve the way MPP computes slave node areas for AUTOMATIC_TIEBREAK contacts (and other that use areas). This should result in less mesh dependency in the failure condition of AUTOMATIC_TIEBREAK contacts. • MPP: synchronize rigid body flags for shared nodes during rigid-to-deformable switching so that these nodes are handled consistently across processors. • Add new pfile decomposition region option “partsets”. Takes a list of part sets (SET_PART) from the keyword input and uses them to define a region. • Apply decomposition transformation (if defined) to: ◦ *CONTROL_MPP_DECOMPOSITION_PARTS_DISTRIBUTE ◦ *CONTROL_MPP_DECOMPOSITION_PARTSET_DISTRIBUTE ◦ *CONTROL_MPP_DECOMPOSITION_ARRANGE_PARTS. • Honor TIEDPRJ flag on *CONTROL_CONTACT for MPP groupable tied interfaces. • Increase initial search distance in MPP tied contact to include slave and master thicknesses. • Tweak MPP_INTERFERENCE contact to better handle deep initial penetrations. INTRODUCTION • MPP: Reorganize how *RIGIDWALL_PLANAR_FORCES is handled, which greatly improves scaling. • Add new MPP pfile option: directory { local_dirs { path1 path2 path3 } which will assign different local working directories to different processors, to balance the I/O load. • Miscellaneous MPP enhancements: ◦ Restructure and reduce memory usage of 3D ALE searching of neighbor- ing algorithm. Now, the code can handle hundreds of millions ALE ele- ments during decomposition. ◦ Support *PARTICLE_BLAST. ◦ Support SPH 2D contact. ◦ Greatly speed up reconstruction of eroding contact surface, (soft = 0,1) when using large number of cores. • Add the following options for small restarts: ◦ *CHANGE_VELOCITY_GENERATION, ◦ *CHANGE_RIGIDWALL_option, ◦ PSNFAIL option to *CONTROL_SHELL • MPP full deck restart: Restore behavior consistent with SMP which is that only the nodes of materials being initialized (not all nodes) are initialized from d3full. • MPP: add full deck restart support for AUTOMATIC_TIEBREAK contact types. • Implement *DELETE_PART for seatbelt parts. The associated slipring, retractors and pretensioners will be deactivated as well. • Add support for MPP restarts with USA coupling. • Add NREP option to *SENSOR_CONTROL to repeat NREP cycles of switches given on Card 2. • Implement *SENSOR_CONTROL TYPEs BELTPRET, BELTRETRA and BELT- SLIP control the pretensioners, retractors and sliprings of a 2D seatbelt. • Add function SENSORD to *DEFINE_CURVE_FUNCTION to return the value of a sensor. • Replace *SENSOR_DEFINE_ANGLE with more general *SENSOR_DEFINE_- MISC. MTYPEs include ANGLE, RETRACTOR, RIGIDBODY, and TIME. • Add rcforc output for *CONTACT_2D_NODE_TO_SOLID (supported for ASCII output only; not binout). • Add temperature output (when applicable) to sphout file (*DATABASE_SPHO- UT). INTRODUCTION • Add support of *MAT_ALE_VISCOUS for SPH particles. This allows modeling of non-viscous fluids with constant or variable viscosity, i.e, non-newtonian type fluid using SPH. • Add support of *EOS for *MAT_272 with SPH particles. • Add support of *MAT_255, *MAT_126, and *MAT_26 (with AOPT = 2 only) for SPH particles. • Add new keyword command *SECTION_SPH_INTERACTION: Combined with CONT = 1 in *CONTROL_SPH card, this keyword is used to define the partial interaction between SPH parts through normal interpolation method and partial interaction through the contact option. All the SPH parts defined through this keyword will interact with each other through normal interpolation method automatically. • Add support for *DATABASE_TRACER for axisymmetric SPH (IDIM = -2 in *CONTROL_SPH). • ICONT in *CONTROL_SPH now affects *DEFINE_SPH_TO_SPH_COUPLING in the sense of enabling or disabling the coupling for deactivated particles. • The commands *STOCHASTIC_TBX_PARTICLES and *CHEMISTRY_CON- TROL_TBX are now available for use (along with the CESE solver) in TBX-based explosives simulations. • Multi-nozzle injection mode is implemented for spray injection. • Add logic to skip thermal computations during dynamic relaxation for a coupled thermal-structual problem (i.e. when SOLN = 2 on the *CONTROL_SOLUTION keyword). This does not affect the use of *LOAD_THERMAL keywords during dynamic relaxation. • Implement *DEFINE_CURVE_FUNCTION for convection, flux, radiation boundary • conditions in thermal-only analyses, both 2D and 3D. • *BOUNDARY_CONVECTION, *BOUNDARY_FLUX, and thermal dynamics are implemented for 20 node brick element. • Include the reading of thermal data to *INCLUDE_BINARY. • Allow *DEFINE_FUNCTION_TABULATED to be used in any place that requires a function of 1 variable. Specifically, as a displacement scale factor with *INTER- FACE_LINKING_NODE. • Add new MUTABLE option for *PARAMETER and *PARAMETER_EXPRES- SION to indicate that it is OK to redefine a specific parameter even if *PARAME- TER_DUPLICATION says redefinition is not allowed. Also, only honor the first *PARAMETER_DUPLICATION card. INTRODUCTION • Add functions DELAY and PIDCTL to *DEFINE_CURVE_FUNCTION for simulating PID (proportional-integral-derivative) controllers. • *DEFINE_TABLE: Add check of table's curves for mismatching origin or end points. • Update ANSYS library to version 16.0. • Enhance report of "Elapsed time" in d3hsp. • Add keyword *INCLUDE_UNITCELL to create a keyword file containing user- defined unit cell information with periodic boundary conditions. • Add *INCLUDE_AUTO_OFFSET: the node and element IDs of the include file will be checked against IDs of the previously read data to see if there is any duplication. If duplicates are found, they will be replaced with another unique ID. Capabilities added to create LS-DYNA R9.0: See release notes (published separately) for further details. • *AIRBAG ◦ Disable CPM airbag feature during DR and reactivate in the transient phase. ◦ *AIRBAG_WANG_NEFSKE_POP_ID pop venting based on RBIDP is now supported correctly (MPP only). ◦ *AIRBAG_INTERACTION: Fixed MPP airbag data sync error to allow final pressure among in- teracted airbags to reach equilibrium. ◦ *AIRBAG_PARTICLE: When IAR = -1 and Pbag or Pchamber is lower than Patm, ambient air will inflate the bag through external vents and also fabric porosity. Treat heat convection when chamber is defined. Output pres+ and pres- to CPM interface forces file for internal parts. Allow IAIR = 4 to gradually switch to IAIR = 2 to avoid instability. Allow using shell to define inflator orifice. The shell center and nor- mal will be used as orifice node and flow vector direction. Bug fix for porous leakage for internal fabric parts using CPM. New feature to collect all ring vents into a single vent in order to cor- rectly treat enhanced venting option. All the vent data will only be output to the first part defined in the part set. INTRODUCTION Evaluate airbag volume based on relative position to avoid trunca- tion. The bag volume becomes independent of coordinate transfor- mation. Support explicit/implicit switch and dynamic relaxation for *AIRBAG_PARTICLE. Support vent/fabric blockage for CPM and ALE coupled analysis. New option in *CONTROL_CPM to allow user defined smoothing of impact forces. Fixed bug affecting *AIRBAG_PARTICLE_ID with PGP encryption. • *ALE ◦ *ALE_REFERENCE_SYSTEM_GROUP: For prtype = 4, allow the ALE mesh to follow the center of mass of a set of nodes. ◦ *CONTROL_ALE: Add a variable DTMUFAC to control the time step related to the vis- cosity from *MAT_NULL (if zero, the viscosity does not control the time step). Implement a 2D version of BFAC and CFAC smoothing algorithm. ◦ *ALE_SMOOTHING: Automatically generate the list of 3 nodes for the smoothing constraints and implement for MPP. ◦ *SECTION_ALE2D, *SECTION_SOLID_ALE: Allow a local smoothing controlled by AFAC,...,DFAC. ◦ *ALE_SWITCH_MMG: Allow the variables to be modified at the time of the switch. ◦ *CONTROL_REFINE_ALE: Add a variable to delay the refinement after removal (DELAYRGN), one to delay the removal after the refinement (DELAYRMV), and one to prevent any removal in a certain radius around latest refinements (RADIUSRMV). ◦ *ALE_STRUCTURED_MESH: Implemented structured ALE mesh solver to facilitate rectilinear mesh generation and to run faster. • *BOUNDARY ◦ *BOUNDARY_AMBIENT_EOS: Implement *DEFINE_CURVE_ FUNCTION for the internal energy and relative volume curves. ◦ *BOUNDARY_AMBIENT: Apply ambient conditions to element sets. ◦ Fix for adaptivity dropping SPCs in some cases (MPP only). ◦ Added conflict error checking between rigid body rotational constraints (*CONSTRAINED_JOINT) with joints between rigid bodies and *BOUNDARY_PRESCRIBED_ORIENTATION. ◦ The first rigid body of the prescribed orientation cannot have any rotation- al constraints. Only spherical joints or translational motors can be used be- tween the two rigid bodies of the prescribed orientation. For now explicit INTRODUCTION will be allowed to continue with these as warnings.Implicit will terminate at end of input checking. ◦ Instead of error terminating with warning message, STR+1371, when *BOUNDARY_PRESCRIBED_MOTION and *BOUNDARY_SPC are ap- plied to same node and dof, issue warning message, KEY+1106, and re- lease the conflicting SPC. ◦ Fix erroneous results if *SET_BOX option is used for *BOUNDARY_ PRESCRIBED_MOTION. ◦ Fix *BOUNDARY_PRESCRIBED_ACCELEROMETER_RIGID for MPP. It may error terminate or give wrong results if more than one of this key- word are used. ◦ Fix segmentation fault when using *BOUNDARY_PRESCRIBED_ ORIENTATION with vad = 2, i.e. cubic spline interpolation. ◦ Fix incorrect behavior PLANE, i.e. > 1, are used. if multiple *BOUNDARY_SPC_SYMMETRY_ ◦ Fix incorrect motion if *BOUNDARY_PRESCRIBED_MOTION_RIGID_ LOCAL is on a rigid part which is merged with a deformable part that has been switched to rigid using *DEFORMABLE_TO_RIGID. ◦ Fix incorrect external work when using *BOUNDARY_PRESCRIBED_ MOTION with or without_RIGID option. The dof specified in *BPM was not considered when computing the external work. Also, when multiple *BPM applied to the same node/rigid body with different dof may also cause incorrect computation of external work. incorrect velocities when using *BOUNDARY_PRESCRIBED_ MOTION_RIGID_LOCAL and *INITIAL_VELOCITY_RIGID_BODY for rigid bodies. ◦ Fix ◦ Implement check for cases where *MAT_ACOUSTIC nodes are merged with structural nodes on both sides of a plate element and direct the user to the proper approach to this situation - *BOUNDARY_ACOUSTIC_ COUPLING. ◦ *BOUNDARY_ACOUSTIC_COUPLING with unmerged, coincident node coupling now implemented in MPP. ◦ MPP logic corrected so *MAT_ACOUSTIC and *BOUNDARY_ ACOUSTIC_COUPLING features may be used with 1 MPP processor. ◦ Fixed bug for *BOUNDARY_PRESCRIBED_MOTION if part label option is used. • BLAST ◦ Improve *LOAD_BLAST_ENHANCED used with ALEPID option in *LOAD_BLAST_SEGMENT: ◦ Rearrange the ambient element type 5 and its adjacent element into same processor to avoid communications. ◦ Eliminate several n-by-n searches for segment set and ambient type 5 with its neighboring elements to speed up the initialization. INTRODUCTION ◦ Change the name of keyword *DEFINE_PBLAST_GEOMETRY to *DEFINE_PBLAST_HEGEO. Both names will be recognized. • *CESE (Compressible Flow Solver) ◦ Modified the CESE moving mesh CHT interface condition calculation to deal with some occasional MPP failures that could occur with mesh corner elements. ◦ Improved the CESE spatial derivatives approximation in order to bring better stability to the CESE solvers. ◦ The 3D SMP and MPP CESE immersed boundary solvers now work with structural element erosion. ◦ A new energy conservative conjugate heat transfer method has been added to the following 2D and 3D CESE Navier-Stokes equation solvers: Fixed mesh (requires use of *CESE_BOUNDARY_CONJ_HEAT input cards) Moving mesh FSI Immersed boundary FSI ◦ Prevent the fluid thermal calculation from using too short a distance be- tween the fluid and structure points in the new IBM CHT solvers. ◦ In the under resolved situation, prevent the CHT interface temperature from dipping below the local structural node temperature. ◦ Add detection of blast wave arrival at CESE boundary condition face first sensing the leading edge of the pulse (used with *LOAD_BLAST_ ENHANCED). ◦ Set CESE state variable derivatives to more stable values for the blast wave boundary condition. ◦ Corrected time step handling for the CESE Eulerian conjugate-heat transfer solver. This affected only the reported output time. ◦ Added CESE cyclic BC capability to the moving mesh CESE solver. ◦ Fixed some issues with 2D CESE solvers where the mesh is created via *MESH cards. ◦ For the CESE solver coupled with the structural solver (FSI), corrected the time step handling. ◦ For the CESE mesh motion solvers, and the ICFD implicit ball-vertex mesh motion solver, added a mechanism to check if all of the imposed boundary displacements are so small that it is not necessary to actually invoke the mesh motion solver. This is determined by comparing the magnitude of the imposed displacement at a node with the minimum distance to a virtu- al ball vertex (that would appear in the ball-vertex method). The relative scale for this check can be input by the user via field 4 of the *CESE_ CONTROL_MESH_MOV card. INTRODUCTION ◦ Changed the NaN check capability for the CESE solvers to be activated on- ly upon user request. This is input via a non-zero entry in field 7 of the *CESE_CONTROL_SOLVER card. ◦ Much like the ICFD solver, added a mechanism to adjust the distance used by the contact detection algorithm for the *CESE_BOUNDARY_FSI cards, as well as the new moving mesh conjugate heat transfer solvers. This is available through field 6 of the *CESE_CONTROL_SOLVER card. ◦ Added a correction to the moving mesh CESE solver geometry calculation. ◦ Corrected the initial time step calculation for both the 2D and 3D moving mesh CESE solvers. ◦ For the moving mesh CESE solver, replaced the all-to-all communication for fsi quantities with a sparse communication mechanism. • *CHEMISTRY ◦ The immersed boundary FSI method coupled with the chemistry solver is released. Only Euler solvers, both in 2D and 3D, are completed with full chem- istry. Using this technique, CESE FSI Immerged Boundary Method coupled to the chemistry solver can be applied to high speed combustion problems such as explosion, detonation shock interacting with struc- tures, and so on. Some examples are available on our ftp site. • *CONTACT ◦ Fix MPP groupable contact problem that could in some cases have oriented the contact surfaces inconsistently. ◦ Fix bug in *CONTACT_AUTOMATIC_SURFACE_TO_SURFACE_TIED_ WELD. ◦ Fix seg fault when using *CONTACT_AUTOMATIC_SINGLE_SURFACE_ TIED with consistency mode, .i.e. ncpu < 0, for SMP. ◦ Fix false warnings, SOL+1253, for untied nodes using *CONTACT_ AUTOMATIC_SURFACE_TO_SURFACE_TIEBREAK and *CONTACT_ AUTOMATIC_ONE_WAY_SURFACE_TO_SURFACE_TIEBREAK. ◦ Fix *CONTACT_TIED_SHELL_EDGE_TO_SURFACE when rigid nodes are not tied even when ipback = 1. This applies to SMP only. ◦ Issue warning if SOFT = 4 is used with an unsupported contact type, and reset it to 1. ◦ Change "Interface Pressure" report in intfor file from abs(force/area) to - force/area, which gives the proper sign in case of a tied interface in ten- sion. INTRODUCTION ◦ Increase MPP contact release condition for shell nodes that contact solid elements in SINGLE_SURFACE contact. ◦ Fix for MPP IPBACK option for creating a backup penalty-based tied con- tact. ◦ Fix for MPP orthotropic friction in contact. ◦ Fix for MPP *CONTACT_SLIDING_ONLY that was falsely detecting con- tact in some cases. ◦ Skip constraint based contacts when computing the stable contact time step size. ◦ Add error trap if node set is input for slave side of single surface contact. ◦ MPP: some fixes for constrained tied contact when used with adaptivity. The behavior of the slave nodes in adaptive constraints was not correct if they were also master nodes of a tied interface. This has been fixed, and support for the rotations required for CONTACT_SPOTWELD have also been added. ◦ MPP: update to AUTOMATIC_TIEBREAK option 5 to release the slave nodes (and report them as having failed) when the damage curve reaches 0. ◦ Fix made to routine that determines the contact interface segments, which was not handling pentahedral thick shell elements correctly. ◦ MPP: fix for strange deadlock that could happen if a user defines a *CONTACT_FORCE_TRANSDUCER that has no elements in it and so gets deleted. ◦ MPP contact: add support for *DEFINE_REGION to define an active con- tact region. Contact occurring outside this region is ignored. This is only for MPP contact types: AUTOMATIC_SINGLE_SURFACE AUTOMATIC_NODES_TO_SURFACE AUTOMATIC_SURFACE_TO_SURFACE AUTOMATIC_ONE_WAY_SURFACE_TO_SURFACE ◦ MPP fix for table based friction in non-groupable contact. ◦ MPP: add frictional work calculation for beams in *CONTACT_ AUTOMATIC_GENERAL. ◦ Added new option "FTORQ" for contact. Currently implemented only for beams in *CONTACT_AUTOMATIC_GENERAL in MPP. Apply torque to the nodes to compensate for the torque introduced by friction. Issue error message when users try to use SOFT = 2/DEPTH = 45 contact for solid el- ements. ◦ R-adaptivity, ADPOPT = 7 in *CONTROL_ADAPTIVE, is now available for SMP version of *CONTACT_SURFACE_TO_SURFACE,_NODES_TO_ SURFACE,_AUTOMATIC_SURFACE_TO_SURFACE, and_ AUTOMATIC_NODES_TO_SURFACE (SOFT = 0 or 1 only). INTRODUCTION ◦ The options AUTOMATIC_SURFACE_TO_SURFACE_COMPOSITE has been added to model composite processing. The same option may be used to model certain types of lubrication, and AUTOMATIC_SURFACE_TO_ SURFACE_LUBRICATION may be used instead of the COMPOSITE op- tion for clarity. (The two keyword commands are equivalent.) ◦ Added AUTOMATIC_SURFACE_TO_SURFACE_TIED_WELD to model the simulation of welding. As regions of the surfaces are heated to the welding temperature and come into contact, the nodes are tied. ◦ Added *CONTACT_TIED_SHELL_EDGE_TO_SOLID. This contact transmits the shell moments into the solid elements by using forces unlike the SHELL_EDGE_TO_SURFACE contact with solid elements. This capa- bility is easier for users than *CONSTRAINED_SHELL_TO_SOLID. The input is identical to *CONTACT_TIED_SHELL_EDGE_TO_SURFACE (ex- cept for the keyword). ◦ Fix incorrect motion of displayed rigidwall between 0.0 < time < birth_time when birth time > 0.0 for *RIGIDWALL_GEOMETRIC_FLAT_MOTION_ DISPLAY. The analysis was still correct. Only the displayed motion of the rigidwall is incorrect. ◦ Fix corrupted intfor when using parts/part sets in *CONTACT_ AUTOMATIC_.... This affects SMP only. ◦ Fix incorrect stonewall energy when using *RIGIDWALL_PLANAR_ ORTHO. ◦ Fix unconstrained nodes when using *CONTACT_TIED_SURFACE_TO_ in warning message, SURFACE_CONSTRAINED_OFFSET resulting SOL+540. This affects SMP only. ◦ Fix spurious repositioning of nodes when using *CONTACT_SURFACE_ TO_SURFACE for SMP. ◦ Enable MAXPAR from optional card A to be used in *CONTACT_TIED_ SURFACE_TO_SURFACE. It was originally hard-coded to 1.07. ◦ The shells used for visualisation of *RIGIDWALL_PLANAR_MOVING_ DISPLAY and *RIGIDWALL_PLANAR_MOVING_DISPLAY in d3plot were not moving with the rigidwall. This is now fixed. ◦ Fix incorrect frictional forces if_ORTHO_FRICTION is used in *CONTACT_AUTOMATIC_SURFACE_TO_SURFACE. ◦ Fix seg fault when using *CONTACT_ENTITY and output to intfor file with MPP, i.e. s = intfor in command line. ◦ Fix ineffective birth time for *CONTACT_TIED_NODES_TO_SURFACE. ◦ Fix untied contacts when using *CONTACT_TIED... with *MAT_ ANISOTROPIC_ELASTIC_PLASTIC/*MAT_157. ◦ Fix MPP hang up when using *CONTACT_ENTITY. ◦ Allow *CONTACT_AUTOMATIC_GENERAL to use MAXPAR from con- tact optional card A instead of using the hard coded value of 1.02. This will better detect end to end contact of beams. This applies to SMP only. ◦ Fix *CONTACT_TIED_SHELL_EDGE_TO_SURFACE for SMP which ig- nores MAXPAR in contact optional card A. INTRODUCTION ◦ Fix seg fault when using *CONTACT_GUIDED_CABLE. ◦ Fix segmentation fault when using *CONTACT_AUTOMATIC_SINGLE_ SURFACE_TIED in consistency mode, i.e. ncpu < 0 in command line, for SMP. ◦ Fix incorrect contacts when using *CONTACT_AUTOMATIC_GENERAL_ INTERIOR for beams with large differences in thickness and when the thinner beams are closer to each other than to the thicker beams. Affects SMP only. ◦ Fixed force transducers with MPP segment based contact when segments are involved with multiple 2 surface force transducers. The symptom was that some forces were missed for contact between segments on different partitions. ◦ Fixed an MPP problem in segment based contact that cased a divide by ze- ro during the bucket sort. During an iteration of the bucket sort, all active segments were somehow in one plane which was far from the origin such that a dimension rounded to zero. The fix for this should effect only this rare case and have no effect on most models. ◦ Fixed thermal MPP segment based contact. The message passing of ther- mal energy due to friction was being skipped unless peak force data was written to the intfor file. ◦ Fixed MPP segment based implicit contact. A flaw in data handling caused possible memory errors during a line search. ◦ Fixed implicit dynamic friction for segment based contact. For sliding fric- tion, the implicit stiffness was reduced to an infinitesimal value. Also, the viscous damping coefficient is now supported for implicit dynamic solu- tions. ◦ Fixed segment based contact when the data has all deformable parts that are switched to rigid at the start of the calculation and then switched back to deformable prior to contact occurring. A flaw was causing contact to be too soft. This is now corrected. ◦ Fixed a flaw in segment based contact with DEPTH = 25 that could allow penetration to occur. ◦ Improved edge-to-edge contact checking (DEPTH = 5,25,35) and the slid- ing option (SBOPT = 4,5) in areas where bricks have eroded when using segment based eroding contact. ◦ Improved the initial penetration check (IGNORE = 2 on *CONTROL_ CONTACT) of segment based contact to eliminate false positives for shell segments. Previously, the search was done using mid-plane nodes and the gap or penetration adjusted to account for segment thicknesses after. The new way projects the nodes to the surface first and uses the projected sur- face to measure penetration. For brick segments with zero thickness there should be no difference. For shell segments, the improved accuracy will me more noticeable for thicker segments. ◦ Improved segment based contact when SHAREC = 1 to run faster when there are rigid bodies in the contact interface. INTRODUCTION ◦ Fixed a possible problem during initialization of segment based contact. Options that use neighbor segment data such as the sliding option and edge-to-edge checking could access bad data if the same nodes were part of both the slave and master surfaces. This would not be a normal occur- rence, but could happen. ◦ Updated segment based contact to improve accuracy at points away from the origin. The final calculations are now done with nodal and segment lo- cations that have been shifted towards the origin so that coordinate values are small. ◦ The reporting of initial penetrations and periodic intersection reports by segment based contact was corrected for MPP solutions which were report- ing incorrect element numbers. ◦ Fixed memory errors in 2D automatic contact initialization when friction is used. ◦ Fixed 2D force transducers in the MPP version which could fail to report master surface forces. Also fixed 2 surface 2D force transducers when the smp parallel consistency option is active. ◦ Fixed *CONTACT_2D_AUTOMAITC_SINGLE_SURFACE and SUR- FACE_TO_SURFACE which could exhibit unpredictable behavior such as a force spike or penetration. ◦ Fixed a serious MPP error in the sliding option of *CONTACT_2D_ AUTOMATIC that could lead to error termination. ◦ Fixed a problem with birth time for *CONTACT_2D_AUTOMATIC_TIED when used with sensor switching. Also, fixed a problem in the contact en- ergy calculation that could lead to abnormal terminations. Finally, I made the process of searching for nodes to tie more robust as some problem was found with nodes being missed. ◦ Fixed a 2D automatic contact bug that occurred if a segment had zero length. An infinite thickness value was calculated by A/L causing the bucket sort to fail. ◦ Added support for *CONTACT_ADD_WEAR for smp and mpp segment based (SOFT = 2) contact. This option enables wear and sliding distance to be measured and output to the intfor file. ◦ Added support to segment based contact for the SRNDE parameter on op- tional card E of *CONTACT. ◦ Added support to segment based eroding contact for SBOXID and MBOX- ID on card 1 of *CONTACT. ◦ Added support for *ELEMENT_SOURCE_SINK used with segment based contact. With this update, inactive elements are no longer checked for con- tact. ◦ Added a segment based contact option to allow the PSTIFF option on *CONTROL_CONTACT to be specified for individual contact definitions. The new parameter is PSTIFF on *CONTACT on optional card F, field 1. Prior to this change, setting PSTIFF on *CONTROL_CONTACT set all con- tact to use the alternate penalty stiffness method. With this update, PSTIFF INTRODUCTION on *CONTROL_CONTACT now sets a default value, and PSTIFF on card F can be used to override the default value for an individual contact inter- face. ◦ Added support for REGION option on optional card E of *CONTACT when using segment based, SOFT = 2 contact. This works for all support- ed keywords, SMP and MPP. ◦ Added master side output in the MPP version for 2-surface force transduc- ers when used with segment based (soft = 2) contact. ◦ Added contact friction energy to the sleout database file for _2D_AUTOMATIC_SURFACE_TO_SURFACE and _2D_AUTOMATIC_SINGLE_SURFACE contact. ◦ Enabled segment based contact (SMP and MPP) to work with type 24 (27- node) solid elements. ◦ Enabled the ICOR parameter on *CONTACT, optional card E to be used with segment based (SOFT = 2) contact. ◦ Fixed output to d3hsp for *CONTACT_DRAWBEAD using negative curve ID for LCIDRF ◦ Add slave node thickness and master segment thickness as input argu- ments to the *USER_INTERFACE_FRICTION subroutine usrfrc (SMP). ◦ Forming mortar contact can now run with deformable solid tools and hon- ors ADPENE to account for curvatures and penetrations in adaptive step. This applies to h- as well as r-adaptivity. ◦ Single surface and surface-to-surface mortar contact accounts for rotational degrees of freedom when contact with beam elements. This allows for beams to "roll" on surfaces and prevents spurious friction energy to be generated when in contact with rotating parts. ◦ Maximum allowable penetration in forming and automatic mortar contacts is hereforth .5*(tslav+tmast)*factor where tmast = thickness of slave seg- ment and tmast = thickness of master segment. The factor is hardwired to 0.95, but is subject to change. Prior to this it was .5*tslav, which seems in- adequate (too small) in coping with initial penetrations in automotive ap- plications using standard modeling approaches. ◦ Up to now, mortar contact has only acted between flat surfaces, now ac- count is taken for sharp edges in solid elements (the angle must initially be larger than 60 degrees), may have to increase the corresponding stiffness in the future. ◦ When solid elements are involved in mortar contact the default stiffness is increased by a factor of 10. This is based on feedback from customers indi- cating that the contact behavior in those cases has in general been too soft. This may change the convergence characteristics in implicit but the results should be an improvement from earlier versions. ◦ The OPTT parameter on *PART_CONTACT for the contact thickness of beams is now supported in mortar contact. INTRODUCTION ◦ *CONTACT_ADD_WEAR: A wear law, Archard's or a user defined, can be associated with a contact interface to assess wear in contact. By specifying WTYPE < 0 a user defined wear subroutine must be written to customize the wear law. For the Archard's wear law, parameters can depend on con- tact pressure, relative sliding velocity and temperature. Contacts support- ed are *CONTACT_FORMING_SURFACE_TO_SURFACE, *CONTACT_ FORMING_ONE_WAY_TO_SURFACE and *CONTACT_AUTOMATIC_ SURFACE_TO_SURFACE. To output wear data set NWEAR = 1 or NWEAR = 2 on *DATABASE_EXTENT_INTFOR. If NWEAR is set to 2 then the sliding distance is output to the intfor file, in addition to the wear depth. Otherwise only wear depth is output. Also, the parameter NWUSR specifies the number of user wear history variables to be output in case a user defined wear routine is used. By specifying CID (contact interface id) to a negative number, the wear depth will couple to the contact in the sim- ulation in the sense that the penetration is reduced with wear. The effect is that contact pressure will be redistributed accordingly but is only valid for relatively small wear depths. A formulation for larger wear depths lie in the future which will require modification of the actual geometry. ◦ Fixed bug affecting *CONTACT_RIGID_NODE_SURFACE (broken at rev. 86847). The bug was in reading *NODE_RIGID_SURFACE. ◦ A bug fix in *CONTACT_DRAWBEAD_INITILIZE. - The bug was caused by a sudden increase in effective strain after the element passed the draw- bead. When the increase in strain is too big, the search algorithm was not working reasonably in the material routine. At the drawbead intersection point, an element could be initialized twice by two bead curves, and cause abnormal thickness distribution. in *CONTACT_FORMING_ONE_WAY_SURFACE_TO_ SURFACE_SMOOTH which removes the limitation that the contact must be defined by segment set. ◦ Fix a bug ◦ SMOOTH option does not apply to FORMING_SURFACE_TO_SURFACE contact. When the SMOOTH option is used, we now write a warning mes- sage and disregard the SMOOTH option. • *CONSTRAINED ◦ *CONSTRAINED_LAGRANGE_IN_SOLID: Implement *CONSTRAINED_LAGRANGE_IN_SOLID_EDGE in 2D. ◦ Fixed bug in *DAMPING_RELATIVE. If the rigid part PIDRB is the slave part in *CONSTRAINED_RIGID_BODIES, the damping card did not work correctly. There is a work-around for previous LS-DYNA versions: set PIDRB to the master part in *CONSTRAIEND_RIGID_BODIES, not the slave part. ◦ *CONSTRAINED_RIGID_BODY_INSERT: This keyword is for modeling die inserts. One rigid body, called slave rigid body, is constrained to move INTRODUCTION with another rigid body, called the master rigid body, in all directions ex- cept for one. ◦ A variety of enhancements for *CONSTRAINED_INTERPOLATION. Enhanced the error message when nodes involved in the constraint have been deleted. for row Removed printing of 0 node ID in MPP. Added a warning if there are too many (now set at 1000) nonzeroes in a constraint *CONSTRAINED_INTERPOLATION or *CONSTRAINED_LINEAR to protect implicit's constraint processing. These constraints will be processed differently in future releases. We modified the constraint processing software to robustly handle con- straint rows with thousands of nonzero entries. We added error checking for co-linear independent nodes as these constraints allow singularities in the model. ◦ Improved implicit's treatment of the constraints for *CONSTRAINED_ BEAM_IN_SOLID. ◦ Added error checking on the values of the gear ratios in *CONSTRAINED_ JOINTS. ◦ *CONSTRAINED_BEAM_IN_SOLID: Thick shell elements supported. Wedge elements supported. Debonding law by user-defined subroutine (set variable AX- FOR > 1000). Debonding law by *DEFINE_FUNCTION (set variable AXFOR < 0). ◦ Error terminate with message, SOL+700, if CIDA and CIDB is not defined for *CONSTRAINED_JOINT_STIFFNESS_GENERALIZED. ◦ Fix incorrect constraints on rotary dof for adaptivity. ◦ Fix incorrect motion in *DEFORMABLE_TO_RIGID_ AUTOMATIC and if any of the *CONSTRAINED_NODAL_RIGID_BODY nodes belongs to a solid element. if NRBF = 2 ◦ Fix input error when using large load curve ID for FMPH, FMT, FMPS in card 3 of *CONSTRAINED_JOINT_STIFFNESS with_GENERALIZED or_ TRANSLATIONAL options. ◦ Fix seg fault if using tables for FMPH of *CONSTRAINED_JOINT_ STIFFNESS and if the angle of rotation is less than the the abscissa of the table or load curves. ◦ Fixed an problem with *CONSTRAINED_BEAM_IN_SOLID when used in a model that also uses segment based eroding contact in the MPP version. This combination now works. INTRODUCTION ◦ Improved the precision of spot weld constraints (*CONSTRAINED_ SPOTWELD) to prevent possible divide by zeroes when the inertia tensor is inverted. This affects the single precision version only. ◦ Fix for damage SPOTWELD, MODEL = 2. function in *CONSTRAINED_INTERPOLATION_ ◦ Add some user-friendly output (rigid body id) to d3hsp for *CONSTRAINED_NODAL_RIGID_BODY_INERTIA. ◦ Add new option to *CONSTRAINED_SPR2 to connect up to 6 shell ele- ment parts (metal sheets) with only one rivet location node. This is in- voked by defining extra part IDs for such a multi-sheet connection. ◦ Add more flexibility to *CONSTRAINED_SPR2: Load curve function ex- ponent values originally hardwired as "8" can now be defined with new input parameters EXPN and EXPT. ◦ Fixed bug wherein the joint ID in *CONSTRAINED_JOINT_COOR was read incorrectly. ◦ Fixed duplicate ID for *CONSTRAINED_SPOTWELD, ..._NODE_SET,_ POINTS and_SPR2. ◦ Fix keyword SPR4 INTERPOLATION_SPOTWELD, where BETA2 was replaced by BETA3. ◦ Significantly reduce the memory demand in the initialization stage of *CONSTRAINED_ option reader for in *CONSTRAINED_MULTIPLE_GLOBAL for implicit analysis. ◦ The unit cell mesh and constraint generated by *INCLUDE_UNITCELL now supports job ID. • *CONTROL ◦ Terminate and print error KEY+1117 for cases that use *INCLUDE_ TRANSFORM in 3d r-adaptvity. More work is needed to make this com- bination work. ◦ Changed SOL+41 message ("reached minimum step") from an error to a warning and terminate normally. This message is triggered when the DTMIN criterion set in *CONTROL_TERMINATION is reached. ◦ Fixed bug in which h-adaptivity missed some ADPFREQ-based adapta- tions when IREFLG < 0 (*CONTROL_ADAPTIVE). ◦ Fixed bug: MS1ST in *CONTROL_TIMESTEP causes non-physical large mass and inertia on Nodal Rigid Bodies if Dynamic Relaxation is active. The error occurs at the start of the transient solution. The mass can become very large, so the model may appear to be over-restrained. ◦ Add new input check for curves. After rediscretizing curves, check to see how well the original values can be reproduced. If the match is poor, write out See variable CDETOL in *CONTROL_OUTPUT. ◦ Added the ability to specify unique values LCINT for each curve, which override the value set in *CONTROL_SOLUTION. Note: the largest value of LCINT that appears will be used when allocating memory for each load INTRODUCTION curve, so a single large value can cause significant increases in the memory required for solution. ◦ The DELFR flag in *CONTROL_SHELL has new options for controlling the deletion of shell elements. This feature is aimed at eliminating single, de- tached elements and/or elements hanging on by one shared node. ◦ Fix spurious deletion of elements when using TSMIN.ne.0.0 in *CONTROL_TERMINATION, ERODE = 1 in *CONTROL_TIMESTEP and initialized implicitly in dynamic relaxation. ◦ Fix spurious error, STR+755, if using *DAMPING_FREQUENCY_RANGE with *CONTROL_ADAPTIVE. ◦ Add new feature to *CONTROL_SOLUTION, LCACC, to truncate load curve to 6 significant figures for single precision & 13 significant figures for double precision. The truncation is done after applying the offset and scale factors. ◦ Fix "*** termination due to mass increase ***' error when using mass scal- ing with *ELEMENT_MASS_PART. ◦ Fix input error 'node set for nodal rigid body # not found' when using *PART_INERTIA with *CONTROL_SUBCYCLE. ◦ Fixed the negative DT2MS option on *CONTROL_TIMESTEP for thick shell types 5, 6, and 7. ◦ Fixed bug in *CONTROL_CHECK_SHELL if PSID.lt.0 (part set ID) is used ◦ Add new option NORBIC to *CONTROL_RIGID to bypass the check of rigid body inertia tensors being too small. ◦ Add new option ICRQ to *CONTROL_SHELL for continuous treatment of thickness and plastic strain across element edges for shell element types 2, 4, and 16 with max. 9 integration points through the thickness. ◦ Add new option ICOHED to *CONTROL_SOLID. If this value is set to 1, solid cohesive elements (ELFORM 19-22) will be eroded when neighboring (nodewise connected) shell or solid elements fail. ◦ Beam release conditions are now properly supported in selective mass scaling, see IMSCL on *CONTROL_TIMESTEP. ◦ Modified MSGMAX in *CONTROL_OUPUT: MSGMAX Maximum num- ber of each error/warning message > 0 number of message to screen output, all messages written to messag/d3hsp < 0 number of messages to screen output and message/d3hsp = 0 the defaul is 50 ◦ Fix bugs in 3D solid adaptivity (*CONTROL_ADAPTIVE,ADPOPT = 7) so that the solid adaptivity will still work when there are any of the following in the model: thick shells (*SECTION_TSHELL), massless nodes, INTRODUCTION *LOAD_SEGMENT_{option}. ◦ Added PARA = 2 to *CONTROL_PARALLEL which actives consistent for force assembly in SMP. An efficient parallel algorithm is implemented for better perfor- mance when the consistency flag is turned on. It shows better scaling with more cpus. This option is overridden by parameter "para=" on the execu- tion line. parallel • DEM(Discrete Element Method) ◦ Added output of following DES history variables to d3plot: nodal stress and force pressure density force chain damage calculation when *DEFINE_DE_BOND is defined ◦ Added output of following DES history variables to demtrh (*DATABASE_TRACER_DE): coordination number porosity and void ratio stress pressure density ◦ Output ASCII format for demrcf if BINARY.eq.3. ◦ Implement gauss distribution of DE sphere radius for *DEFINE_DE_ INJECTION. The mean radius is 0.5*(rmin+rmax) and standard deviation is 0.5*(rmax-rmin). ◦ For DE sphere, implement the stress calculation for REV (Representative Elementary Volume) using *DATABASE_TRACER_DE and specific RA- DIUS. ◦ Add *BOUNDARY_DE_NON_REFLECTING for defining non-reflecting boundary conditions for DE spheres. ◦ For *CONTROL_DISCRETE_ELEMENT, add the option to create the liq- uid bridge if the initial distance between two DE spheres is smaller than predefined gap. ◦ Added *DATABASE_DEMASSFLOW, see *DEFINE_DE_MASSFLOW_ PLANE, for measuring the mass flow of DE spheres through a surface. The surface is defined by part or part set. Output file is 'demflow'. ◦ Add *DEFINE_DE_INJECTION_ELLIPSE, to define a circular or elliptical injection plane. INTRODUCTION ◦ Add *DEFINE_PBLAST_AIRGEO for *PARTICLE_BLAST which defines initial geometry for air particles. ◦ Add DEM stress calculation when coupling with segment (*DEFINE_DE_ TO_SURFACE_COUPLING). ◦ Fix error in demtrh file output (Window platform only). • EFG (Element Free Galerkin) ◦ Fix bug for ELFORM = 41 implicit when there are 6-noded/4-noded ele- ments. • *ELEMENT ◦ Fix a 2d seatbelt bug triggered by having both 1d and 2d seatbelts, and a 1d pretensioner of type 2, 3 or 9. ◦ Fix MPP bug initializing multiscale spotweld in the unexpected case where the spotweld beam is merged with the shells rather than tied via contact. ◦ Fix bug for *INCLUDE_UNITCELL. ◦ *CONTROL_REFINE_...: Implement the parent-children transition in *CONTACT_2D_SINGLE_SURFACE when a shell refinement occurs. ◦ Fix error traps for *ELEMENT_SEATBELT_... , for example, error termina- tion due to convergence failure in retractors. These error traps worked but could lead to a less graceful termination than other LS-DYNA error traps. ◦ Correct calculation of wrap angle in seatbelt retractor. ◦ Add MPP support for *ELEMENT_LANCING. ◦ *ELEMENT_SEATBELT: Fix a MPP belt bug that can happen when buckle pretensioner is modeled as a type-9 pretensioner. 2D belt and 1D belt now can share the same *MAT_SEATBELT. The section force for 2d belt is recoded to provide more robust and accurate results. The loading curve LLCID of *MAT_SEATBELT can be a table defin- ing strain-rate dependent stiffness curve. IGRAV of *ELEMENT_SEATBELT_ACCELEROMETER can be a curve defining gravitation flag as a function of time. ◦ Add *NODE_THICKNESS to override shell nodal thickness otherwise de- termined via *SECTION_SHELL, *PART_COMPOSITE, or *ELEMENT_ SHELL_THICKNESS. ◦ Fix input error when using *DEFINE_ELEMENT_DEATH with BOXID > 0 for MPP. ◦ Implement subcycling for thick shells. ◦ Fix ineffective *DEFINE_HAZ_PROPERTIES when solid spotwelds and hex spotweld assemblies are both present. INTRODUCTION ◦ Fix incorrect beta written out for *ELEMENT_SHELL_BETA in dynain file when *PART_COMPOSITE keyword is present in the original input. ◦ Fix NaN output to elout_det and spurious element deletion if NO- DOUT = STRAIN or STRAIN_GL or ALL or ALL_GL. ◦ Fix incorrect reading of TIME in card 3 of *ELEMENT_SEATBELT_ SENSOR SBSTYP = 3 when long = s in command line. ◦ *PART_COMPOSITE: Increased the explicit solution time step for thin shell composite elements. The existing method was overly conservative. The new method is based on average layer stiffness and density. ◦ In conjunction with the above change in composite time step calculation, increase nodal inertia in the rare cases of *PART_COMPOSITE in which the bending stability is not satisfied by the membrane stability criterion. The inertia is only increased in the cases where it is necessary; for most models this change has no effect, but this can occur in the case of sandwich sections with stiffer skins around a less stiff core. ◦ Corrected rotational inertia of thin shells when layers have mixed density and the outer layers are more dense than inner layers. The fix will mostly affect elements that are very thick relative to edge length. ◦ Fixed default hourglass control when the *HOURGLASS control card is used but no HG type is specified. We were setting to type 1 instead of 2. Also, fixed the default HG types to match the User's Manual for implicit and explicit. ◦ Fixed the part mass that was reported to d3hsp when *ELEMENT_SHELL_ SOURCE_SINK is used. The inactive elements were being included caus- ing too high mass. ◦ Prevent inactive shell elements (from *ELEMENT_SHELL_SOURCE_ SINK) from controlling the solution time step. ◦ Fixed the reported strain tensor in elements created by *ELEMENT_ SHELL_SOURCE_SINK when strain output is requested. The history was being retained from the previous elements with the same ID. ◦ Fixed torsion in linear beam form 13. A failure to add the torsional mo- ment at node 2 caused an inability to reach equilibrium in the torsional mode. ◦ Fixed solid element 4 so that rigid body translation will not cause strain and stress due to round-off error. ◦ Mixed parallel consistency when used with solid element type 20. A buffer was not being allocated leading to a memory error. ◦ Changed the MPP behavior of discrete beams (ELFORM = 6) when at- tached to elements that fail. They were behaving like null beams, in the sense that it was possible for beam nodes to become dead due to attached elements failing, and discrete beams would be no longer visualized even if the beams themselves had not failed. With this change, the MPP discrete beams now behave like other beams in that the beams have to fail before they are removed. MPP and SMP behavior is now consistent. INTRODUCTION ◦ Improved the precision of the type 2 Belytschko Schwer resultant beam to prevent energy growth in single precision. ◦ Fixed the NLOC option on *SECTION_SHELL for the BCIZ triangle ele- ments (ELFORM = 3) and the DKT triangle elements (ELFORM = 17). The offset was scaled by the solution time step so typically the offset was much smaller than expected. ◦ Fixed elout stress output for shell element forms 23 and 24. The in-plane averaging was incorrect causing wrong output. ◦ Changed *ELEMENT_TSHELL so that both the COMPOSITE and BETA options can be read at the same time. Prior to the fix, only the first one would be read. ◦ Fixed all thick shells to work with anisotropic thermal strains which can be defined by *MAT_ADD_THERMAL. Also, this now works by layer for layered composites. ◦ Fixed implicit solutions with thick shells with *MAT_057 when there are also solid elements in the model that use *MAT_057. Thick shells support only the incremental update of the F tensor but a flag was set incorrectly in the material model. ◦ Fixed *MAT_219 when used with thick shell types 3, 5, and 7. A failure to initialize terms for the time step caused a possible wrong time step. ◦ Fixed orthotropic user defined materials when used with thick shell ele- ments. The storing of the transformation matrix was in the wrong location leading to wrong stress and strain. ◦ For thick shell composites that use element forms 5 and 7, the user can now use laminated shell theory along with the TSHEAR = 1 on *SECTION_ TSHELL to get a constant shear stress through the thickness with a compo- site. ◦ Fixed the initialization of *MAT_CODAM2/*MAT_219 when used with thick shell forms 3, 5, or 7. The 3D thick shell routine uses only 2 terms for the transformation and therefore needs unique initialization of the trans- formation data. ◦ Fixed thick shell types 3 and 5 when used in implicit solutions with *MATs 2, 21, 261, and 263. The material constitutive matrix for *MATs 2 and 21 was not rotated correctly causing wrong element stiffness. The constitutive matrix for *MATs 261 and 263 was not orthotropic. Also, for *MAT_021, type 5 thick shell needed some material terms defined to cor- rect the assumed strain. ◦ Fixed thick shell forms 3 and 5 when used in implicit solutions with non- isotropic materials. The stiffness matrix was wrong due to incorrect trans- formations. ◦ Also, fixed the implicit stiffness of thin and thick shells when used with laminated shell (LAMSHT = 3,4,5 on *CONTROL_ACCURACY). Elements were either failing to converge or converging more slowly due to the failure to adjust the stiffness matrix to be consistent with the assumed strain. theory by assumed strain INTRODUCTION ◦ Added support for *ELEMENT_SHELL_SOURCE_SINK to form 2 ele- ments with BWC = 1 on *CONTROL_SHELL. ◦ Fixed the s-axis and t-axis orientation of beam spot welds in the MPP ver- sion when those beam weld elements are defined with a 3rd node. The 3rd node was being discarded prior to initializing the beam orientation so the s and t-axes were being randomly assigned as if the 3rd node had not been assigned. The effect on solutions is likely fairly minimal since beam mate- rial is isotropic and failure typically is too, but may not be. ◦ Added Rayleigh damping (*DAMPING_PART_STIFFNESS) for thick shell formulations 1, 2, and 6. Previously, it was available for only the thick shells that call 3D stress updates, (forms 3 and 5), but now it is available for all thick shell formulations. ◦ Added new SCOOR options for discrete beam section 6 (*SECTION_ BEAM). A flaw was found in how the discrete beam accounts for rigid body rotation when SCOOR = -3, -2, +2, and +3. A correction for this is made and introduced as new options, SCOOR = -13, -12, +12, and +13. A decision was made to leave the existing options SCOOR = -2, +2, -3 and +3 unchanged so that legacy data could run without changes. ◦ Enabled the ELFORM 18 linear DKT shell element to work with *PART_ COMPOSITE and with an arbitrary number of through thickness integra- tion points. It was limited to a single material and 10 Gauss points. ◦ Added the possibility to write *ELEMENT_SOLID_ORTHO into dynain file if requested. To activate this add OPTCARD to *INTERFACE_ SPRINGBACK and set SLDO = 1. ◦ Refine characteristic length calculation for 27-node solid (ELFORM 24). This change may increase the time step substantially for badly distorted el- ements. ◦ Implement selective reduced integration for 27-node solid (ELFORM 24). ◦ Allow part sets to be used in *DEFORMABLE_TO_RIGID_AUTOMATIC. Either PID is defined negative or "PSET" is set in column 3 (D2R) or 2 (R2D). ◦ Add new option STRESS = 2 to *INCLUDE_STAMPED_PART: no stresses and no history variables are mapped with that setting. ◦ New keyword *PART_STACKED_ELEMENTS provides a method to de- fine and to discretize layered shell-like structures by an arbitrary sequence of shell and/or solid elements over the thickness. ◦ The geometric stiffness matrix for the Belytschko beam element type 2 has been extended to include nonsymmetric terms arising from nonzero mo- ments. Provides "almost" quadratic convergence, still some terms missing to be added in the future. Also support a strongly objective version acti- vated by IACC on *CONTROL_ACCURACY. ◦ The geometric stiffness for the Hughes-Liu element type 1 is fixed. ◦ Fix parsing error in *SECTION_BEAM_AISC. • EM (Electromagnetic Solver) INTRODUCTION ◦ Add the new EM 2d axi solver in SMP and MPP for EM solver 1 (eddy cur- rent). It is coupled with the mechanics and thermal solvers. ◦ The new EM 2d can be used with RLC circuits on helix/spiral geometries using *EM_CIRCUIT_CONNECT. ◦ Add EM contact into new EM 2d axi, in SMP and MPP. ◦ Add *EM_BOUNDARY support in new EM 2d axi solver. ◦ Introduce scalar potential in new EM 2d axi. The 2d axi can also be cou- pled with imposed voltage. ◦ Add new keyword *EM_CIRCUIT_CONNECT to impose linear constraints between circuits with imposed currents in 3d solvers. This allows for ex- ample to impose that the current in circuit 1 is equal to the current in cir- cuit 2 even if the 2 corresponding parts are not physically connected. ◦ Add *EM_VOLTAGE_DROP keyword to define a voltage drop between 2 segment sets. This voltage drop constraint is coupled to the contact con- straint so that the contact (voltage drop = 0) has priority over the *EM_ VOLTAGE_DROP constraint. ◦ Add *EM_CONTROL_SWITCH_CONTACT keyword to turn the EM con- tact detection on and off. ◦ NCYCLBEM/NCYCLFEM in *EM_SOLVER_... can now be different than 1 when EM_CONTACT detected. ◦ Add RLC circuit for type 3 solver (resistive heating). ◦ Add computation of mutuals/inductances in 2d axi for output to em_ circuit.dat ◦ Add criteria on autotimestep calculation when R,L,C circuit used to take into account R,L,C period. ◦ Fix keyword counter in d3hsp. ◦ Better and clearer output to terminal screen. ◦ Support jobid for EM ascii file outputs. • Forming ◦ Improvements to trimming: *DEFINE_CURVE_TRIM_NEW: if trim seed node is not defined, we will search a seed node based on nodes from the sheet blank and the inside/outside flag definition for the trimming curves. Map strain tensors to triangular elements after trimming. ◦ Add a new function to the trim of solid elements in normal (3-D) trimming case, related to *DEFINE_CURVE_TRIM_3D. If the trimming curve is close to the bottom side, set TDIR = -1. If the trimming curve is close to the upper side, set TDIR = 1. INTRODUCTION ◦ Add to *ELEMENT_LANCING. Allow parametric expression for variables END and NTIMES. ◦ A bug fix for *CONTROL_FORMING_AUTOPOSITION_PARAMETER_ SET: Fix distance calculation error when the target mesh is too coarse. ◦ Improvements to springback compensations: Output the new trimming curve with *DEFINE_CURVE_TRIM_3D (previously *DEFINE_CURVE_TRIM), so that it can be easily con- verted to IGES curve by LS-PrePost. or used in another trimming cal- culation. Output each curve to IGES format in the following name format: newcurve_scp001.igs, newcurve_scp002.igs, newcurve_scp003.igs, etc. Output change in file "geocur.trm". This update will allow change from *DEFINE_CURVE_TRIM(_3D,_NEW), whatever is used for in- put. ◦ Add a new keyword: *DEFINE_FORMING_CONTACT to facilitate the forming contact definitions. ◦ Add a new keyword *DEFINE_FORMING_CLAMP, to facilitate clamping simulation. ◦ A new feature in mesh fusion, which allows a moving box to control the fusion, only if the center of the elements is inside the box can the elements can be coarsened. Can be used in conjuntion with *DEFINE_BOX_ ADAPTIVE. ◦ Add a new feature to *DEFINE_BOX_ADAPTIVE: Moving box in adaptiv- ity, useful in roller hemming and incremental forming. ◦ In mesh coarsening, if the node is defined in a node set, the connected ele- ments will be kept from being coarsened. Previously, only *SET_NODE_ LIST was supported. Now option *SET_NODE_GENERAL is allowed. ◦ Add a new function: mesh refinement for sandwich part. The top and bot- tom layers are shell elements and the middle layer is solid elements. Set IFSAND to 1 in *CONTROL_ADAPTIVE. Applies to both 8-noded and 6-noded solid elements. Map stress and history variables to the new elements. ◦ New features related BLANKSIZE_DEVELOPMENT: to blank size development *INTERFACE_ Add *INTERFACE_BLANKSIZE_SYMMETRIC_PLANE to define symmetric plane in blank size development Add *INTERFACE_BLANKSIZE_SCALE_FACTOR. For each trim- ming, different scale factors can be used to compensate the blanksize. This is especially useful when the inner holes are small. Includes an INTRODUCTION option of offset the target curve which is useful if multiple target curves (e.g., holes) and formed curves are far from each other. Allow target curve to be outside of the surface of the blank. Add sorting to the mesh so the initial mesh and the formed mesh do not need to have the same sequence for the nodes. Add a new variable ORIENT, set to "1" to activate the new algorithm to potentially reduce the number of iterations with the use of *INTERFACE_BLANKSIZE_SCALE_FACTOR (scale = 0.75 to 0.9). Fix smooth problem along calculated outer boundary. Automatically determine the curve running directions (IOPTION = 2 and -2 now both give the same results). Accept parameteric expression. ◦ A bug fix for springback compensation: *INCLUDE_COMPENSATION_ SYMMETRIC_LINES Fix reading problem of free format in the original coding. ◦ Add a new keyword *CONTROL_FORMING_BESTFIT. Purpose: This keyword rigidly moves two parts so that they maximally coincide. This feature can be used in sheet metal forming to translate and rotate a spring back part (source) to a scanned part (target) to assess spring back predic- tion accuracy. This keyword applies to shell elements only. ◦ Improvements to *CONTROL_FORMING_AUTOCHECK: When IOFFSET = 1, rigid body thickness is automatically offset, based on the MST value defined in *CONTACT_FORMING_ONE_ WAY_SURFACE. Add new variable IOUTPUT that when set to 1 will output the offset rigid tool mesh, and the new output tool file is: rigid_offset.inc. After output the simulation stops. See R9.0 Manual for further details. When both normal check and offset are used, small radius might cause problem for offsetting. The new modification will check the normal again after offsetting the tool When outputting the rigid body mesh, output the bead nodes also. Changes to *CONTROL_FORMING_AUTOCHECK when used to- gether with SMOOTH option: check and fix rigid body bad elements before converting the master part ID to segment set id to be used by SMOOTH option. Set IOUTPUT.eq. 3 to output rigid body mesh before and after offset. Fix problems offseting a small radius to a even smaller radius. Remove T-intersection. ◦ For *CONTROL_IMPLICIT_FORMING, fix output messages in d3hsp that incorrectly identified steps as implicit dynamic when they were actually implicit static. ◦ Improve *CONTROL_FORMING_UNFLANGING: INTRODUCTION Automatically calculate CHARLEN, so user does not need to input it anymore. Allow nonsmooth flange edge. Instead of using preset value of 0.4 (which works fine for thin sheet metal), blank thickness is now used to offset the slave node (flanges) from the rigid body (die). • *FREQUENCY_DOMAIN ◦ *FREQUENCY_DOMAIN_RANDOM_VIBRATION: Fixed a bug in dump- ing d3psd binary database, when both stress and strain are included. ◦ *FREQUENCY_DOMAIN_SSD_ERP: Implemented the Equivalent adiated Power (ERP) computation to MPP. ◦ *FREQUENCY_DOMAIN_ACOUSTIC_BEM: Enabled running dual collocation BEM based on Burton-Miller for- mulation (METHOD = 4) with vibration boundary conditions pro- vided by Steady State Dynamic analysis (*FREQUENCY_DOMAIN_ SSD). Added exponential window function for FFT (FFTWIN = 5). Implemented a new forward and backward mixed radix FFT. Implemented acoustic computation restart from frequency domain boundary conditions, in addition to time domain boundary condi- tions (RESTRT = 1). Enabled out-of-core velocity data storage, to solve large scale prob- lems. Implemented option HALF_SPACE to Rayleigh method (METH- OD = 0) to consider acoustic wave reflection. Added velocity interpolation to take care of mismatching between acoustic mesh and structural mesh (*BOUNDARY_ACOUSTIC_ MAPPING), for the case that the boundary conditions are provided by Steady State Dynamic analysis. Added weighted SPL output to acoustic computation (DBA = 1,2,3,4). Implemented radiated sound power, and radiation efficiency compu- tation to collocation BEMs (METHOD = 3,4). Added new ASCII xy- plot databases Press_Power and Press_radef to save the sound power and radiation efficiency results. Enabled using both impedance and vibration (velocity) boundary conditions in acoustic simulation. ◦ *FREQUENCY_DOMAIN_ACOUSTIC_FEM: Added weighted SPL output to FEM acoustics (DBA = 1,2,3,4). Implemented option EIGENVALUE to perform acoustic eigenvalue analysis; added ASCII database eigout_ac to save acoustic eigenvalue INTRODUCTION results; added binary plot database d3eigv_ac to save acoustic eigen- vectors. Enabled consideration of nodal constraints in acoustic eigenvalue analysis. Enabled FEM acoustic analysis with frequency dependent complex sound speed. Implemented pressure and impedance boundary conditions. ◦ *FREQUENCY_DOMAIN_ACOUSTIC_FRINGE_PLOT: Added this keyword to 1) generate acoustic field points as a sphere or plate mesh (options SPHERE and PLATE), or 2) define acoustic field points mesh based on existing structure components (options PART, PART_SET and NODE_SET) so that user can get fringe plot of acous- tic pressure and SPL. The results are saved in binary plot database d3acs (activated by keyword *DATABASE_FREQUENCY_BINARY_ D3ACS). ◦ *FREQUENCY_DOMAIN_RANDOM_VIBRATION: Changed displacement rms output in d3rms to be the displacement itself, without adding the original nodal coordinates. Implemented von mises stress PSD computation in beam elements. Implemented fatigue analysis with beam elements. Added strain output to binary plot databases d3psd and d3rms, and binout database elout_psd. Added initial damage ratio from multiple loading cases (INFTG > 1). ◦ *FREQUENCY_DOMAIN_SSD: Implemented option ERP to compute Equivalent Radiated Power. It is a fast and simplified way to characterize acoustic behavior of vi- brating structures. The results are saved in binary plot database d3erp (activated by keyword *DATABASE_FREQUENCY_BINARY_ D3ERP), and ASCII xyplot files ERP_abs and ERP_dB. Implemented fatigue analysis based on maximum principal stress and maximum shear stress. • ICFD (Incompressible Flow Solver) ◦ *ICFD_BOUNDARY_FSWAVE: Added a boundary condition for wave generation of 1st order stokes waves with free surfaces. ◦ *ICFD_DATABASE_DRAG_VOL: For computing pressure forces on vol- umes ID (useful for forces in porous domains), output in icfdragivol.dat and icfdragivol.#VID.dat. INTRODUCTION ◦ *ICFD_CONTROL_DEM_COUPLING: Coupling the ICFD solver with DEM particles is now possible. ◦ *ICFD_CONTROL_MONOLITHIC: Added a monolithic solver (=1) which can be selected instead of the traditional fractional step solver (=0). ◦ *ICFD_CONTROL_POROUS: This keyword allows the user to choose be- tween the Anisotropic Generalized Navier-Stokes model (=0) or the Aniso- tropic Darcy-Forchheimer model (=1) (for Low Reynolds number flows). The Monolithic solver is used by default for those creeping flows. ◦ *ICFD_CONTROL_TURBULENCE: Modified existing standard k-epsilon. Added Realizable k-epsilon turbulence model. Added Standard 98 and 06 Wilcox and Menter SST 03 turbulence models. Added Several laws of the wall. Added Rugosity law when RANS turbulence model selected. ◦ *ICFD_MODEL_POROUS: Added Porous model 5 for anistropic materials defined by P-V exper- imental curves. Added porous model 6 for moving domain capabilities for Porous Media volumes using load curves for permeabilities directions. Added porous model 7 for moving domain capabilities for Porous Media volumes using ICFD_DEFINE_POINT for permeabilities di- rections. Added porous model 9 for a new Anisotropic Porous Media flow model (PM model ID = 9): It uses a variable permeability tensor field which is the result of solid dynamic problems. The model reads the solid mesh and the field state and maps elemental permeability ten- sor and solid displacements to the fluid mesh. ◦ *ICFD_MODEL_NONNEWT: Added a few models for non newtonian materials and temperature dependant viscosity : • model 1 : power law non newtonian (now also temperature dependant) • model 2 : carreau fluid • model 3 : cross fluid • model 4 : herschel-bulkley • model 5 : cross fluid II • model 6 : temperature dependant visc (sutherland) • model 7 : temperature dependant visc (power law) INTRODUCTION • model 8 : load curve dependant visc, model 8 is especially interesting since a DEFINE_FUNCTION can be used (for so- lidification applications). ◦ *ICFD_SOLVER_TOL_MONOLITHIC: Used to define atol, rtol, dtol and maxits linear solver convergence controls of the monolithic NS time inte- gration ◦ *MESH_BL: Added support for boundary layer mesh creation by specify- ing the thickness, number of layers, first node near the surface and the strategy to use to divide and separate the elements inside the BL adding. ◦ *ICFD_BOUNDARY_PRESCRIBED_VEL: Added the support of DEFINE_ FUNCTION making the second line of the keyword obsolete. ◦ *ICFD_CONTROL_TIME: Min and Max timestep values can be set. ◦ *ICFD_DATABASE_DRAG: Added frequency output. Added option to output drag repartition percentage in the d3plots as a surface variable. ◦ *ICFD_CONTROL_IMPOSED_MOVE: This keyword now uses *ICFD_ PART and *ICFD_PART_VOL instead of *MESH_VOL for ID. It is now possible to impose a rotation on a part using Euler angles. ◦ *ICFD_CONTROL_OUTPUT: Field 4 now to output mesh in LSPP format and in format to be run by the icfd solver (icfd_fluidmesh.key and icfd_mesh.key) icfd_mesh.key now divides the mesh in ten parts, from best quality element decile to worst. A new mesh is now output at every remeshing. Added support for parallel I/O for Paraview using the PVTU format. ◦ *ICFD_DEFINE_POINT: Points can now be made to rotate or translate. ◦ *ICFD_MAT: Nonnewtonian models and Porous media models are now selected in the third line by using the new ICFD_MODEL keyword family. HC and TC can now be made temperature dependent. ◦ *ICFD_CONTROL_DIVCLEAN: Added option 2 to use a potential flow solver to initialize the Navier Stokes solver. ◦ *ICFD_CONTROL_FSI: Field 5 provides a relaxation that starts after the birthtime. ◦ *ICFD_CONTROL_MESH: Field 3 added a new strategy to interpolate a mesh size during the node insertion. In some cases it speeds up the mesh- ing process and produces less elements. Field 4 changes the meshing strategy in 2d. INTRODUCTION ◦ *ICFD_CONTROL_SURFMESH: Added meshing/adaptation of surface meshing. support for dynamic re- ◦ *ICFD_BOUNDARY_PRESCRIBED_VEL:VAD = 3 now works with DOF = 4. ◦ SF can be lower than 0. ◦ PID can be over 9999 in *ICFD_DATABASE_FLUX. ◦ Fixed d3hsp keyword counter. ◦ Clarified terminal output. ◦ Y+ and Shear now always output on walls rather than when a turbulence model was selected. ◦ Added coordinate of distorted element before remeshing occurs. Output on terminal and messag file ◦ Fixed bug in conjugate heat transfer cases. When an autotimestep was se- lected in *ICFD_CONTROL_TIME, it would always only take the thermal timestep. ◦ An estimation of the CFL number is now output in the d3plot files. This is not the value used for the autotimestep calculation. ◦ Turbulence intensity is now output in the d3plots. ◦ Jobid now supported for ICFD ASCII File outputs. ◦ Fixed communication of turbulent constants in MPP. ◦ Fixed the Near Velocity field output. ◦ Increasing the limit of number of parts for the model. ◦ Temperature added as a surface variable in output. ◦ Fixed non-linear conjugate heat solver. • Implicit ◦ Fixed Implicit for the case of Multi-step Linear (*CONTROL_IMPLICIT_ GENERAL with NSOLVR = 1) with Intermittent Eigenvalue Computation (*CONTROL_IMPLICIT_EIGENVALUE with NEIG < 0). ◦ Recent fix for resultant forces for Multi-step Linear cause segmentation fault when Intermittent Eigenvalue Computation was also active. ◦ Fix possible issue related to constrained contacts in MPP implicit not ini- tializing properly. ◦ Fixed label at beginning of implicit step to be correct for the case of control- load curve (*CONTROL_IMPLICIT_ implicit dynamics via a ling DYNAMICS). ◦ Corrected the computation of modal stresses with local coordinate terms and forsome shell elements . ◦ Corrected *CONTROL_IMPLICIT_INERTIA_RELIEF logic in MPP. In some cases the rigid body modes were lost. ◦ Enhanced implicit's treatment of failing spotwelds (*CONSTRAINED_ SPOTWELD). INTRODUCTION ◦ Added additional error checking of input data for *CONTROL_IMPLICIT_ MODAL_DYNAMICS_DAMPING. ◦ Per user request we added the coupling of prescribed motion constraints for Modal Dynamics by using constraint modes. See *CONTROL_ IMPLICIT_MODAL_DYNAMIC. ◦ Added reuse of the matrix reordering for MPP implicit execution. This will reduce the symbolic processing time which is noticable when using large numbers of MPP processes. Also added prediction of non tied con- tact connections for standard contact and mortar contact. This allows re- use of the ordering when contact interfaces are changing very slightly but can increase the cost of the numerical factorization. Useful only for MPP using large numbers of processes for large finite element models. This re- use checking happens automatically for MPP and is not required for SMP. ◦ Apply improvements to Metis memory requirements used in Implicit MPP. ◦ Enhanced Metis ordering software (ORDER = 2, the default, on *CONTROL_IMPLICIT_SOLVER). ◦ Added new keyword *CONTROL_IMPLICIT_ORDERING to control of features of the ordering methods for the linear algebra solver in MPP Im- plicit. Only should be used by expert users. ◦ The following 4 enhancements are applicable when IMFLAG > 1 on *CONTROL_IMPLICIT_GENERAL. Implicit was modified to reset the time step used in contact when switching from implicit to explicit. Adjusted implicit mechanical time step for the case of switching from explicit to implicit so as not to go past the end time. Explicit with intermittent eigenvalue analysis was getting incorrect results after the eigenvalue analysis because an incorrect time step was used for the implicit computations. For this scenario implicit now uses the explicit time step. The implicit time step is now reset for the dump file in addition to explicit's time. ◦ Implicit's treatment of prescribed motion constraints defined by a box had to be enhanced to properly handle potential switching to explicit. ◦ The following 6 enhancements are for matrix dumping (MTXDMP > 0 on response frequency for *CONTROL_IMPLICIT_SOLVER) (*FREQUENCY_DOMAIN) computations. or ◦ Corrected the collection of *DAMPING_PART_STIFFNESS terms for ele- ments like triangles and 5, 6, and 7 node solid elements. ◦ Corrected Implicit's access of *DAMPING_PART_STIFFNES parameter when triangle and tet sorting is activated. ◦ Fixed Implicit's collecting of damping terms for beams that have reference nodes. INTRODUCTION ◦ There is an internal switch that turns off damping for beams if the run is implicit static. This switch needed to be turned off for explicit with inter- mittent eigenvalue analysis. ◦ Fixed collecting of stiffness damping terms for implicit. Corrected the loading of mass damping terms when collecting damping terms for post processing. ◦ Extend matrix dumping to include dumping the solution vector in addi- tion to the matrix and right-hand-side. ◦ Adjusted Implicit's handling of sw1. and sw3. sense switches to properly handle dumping. If sw1. sense switch is issued when not at equilibrium, then reset time and geometry to that at the end of last implicit time step. If sw3. sense switch is issued, then wait until equilibrium is reached before dumping and continuing. ◦ Enable the use of intermittent eigenvalue computation for models using inertia relief and/or rotational dynamics. See NEIG < 0 on *CONTROL_ IMPLICIT_EIGENVALUE and *CONTROL_IMPLICIT_ROTATIONAL_DYNAMICS. Due to round-off, an implicit intermittent eigenvalue computation was occasionally skipped. A fudge factor of 1/1000 of the implicit time step was added to compen- sate for round-off error in the summation of the implicit time. See NEIG < 0 on *CONTROL_IMPLICIT_EIGENVALUE. *CONTROL_INERTIA_RELIEF and ◦ Added support for *CONSTRAINED_LINEAR for 2D implicit problems. It was already supported for standard 3D problems. ◦ Added warning for implicit when the product of ILIMIT and MAXREF (two parameters on *CONTROL_IMPLICIT_SOLUTION) is too small. For the special case when the user changes the default of ILIMIT to 1 to choose Full Newton and does not change MAXREF then MAXREF is reset to 165 and a warning is generated. Reinstate the option of MAXREF < 0. ◦ Fixed the display of superelements in LS-PrePost. Enhanced reading of Nastran dmig files to allow for LS-DYNA-like comment lines starting with '$'. Fixed a problem with implicit initialization in MPP with 2 or more su- perelements. See *ELEMENT_DIRECT_MATRIX_INPUT. ◦ Turned off annoying warning messages associated with zero contact ele- mental stiffness matrices coming from mortar contact. See *CONTACT_..._ MORTAR ◦ Fixed construction of d3mode file in MPP. Involves proper computation of the reduced stiffness matrix. See *CONTROL_IMPLICIT_MODES ◦ Fixed up *PART_MODES to correctly handle constraint modes. removed rigid body modes correct construction of reduced stiffness matrix ◦ Enhanced the error handling for input for *PART_MODES. ◦ Modified open statements for binary files used by implicit to allow for use of *CASE. INTRODUCTION ◦ Removed internal use files such as spooles.res when not required for de- bugging. ◦ Fixed implicit static condensation and implicit mode computation to properly deal with the *CASE environment. See *CONTROL_IMPLICIT_ STATIC_CONDENSATION and *CONTROL_IMPLICIT_MODES. Sort node/dof sets for implicit_mode to get correct results. Properly handle cases with only solid elements. ◦ Add implicit implementation of the new "last location" feature for MPP er- ror tracking. ◦ Fixed problem with implicit processing of rigid body data with deformable to rigid switching (*DEFORMABLE_TO_RIGID). ◦ Extended Implicit model debugging for LPRINT = 3 (*CONTROL_ IMPLICIT_SOLVER) to isogeometric and other large elemental stiff matri- ces. ◦ Added beam rotary mass scaling to the modal effective mass computation. Enhanced implicit computation of modal effective mass that is output to file eigout with *CONTROL_IMPLICIT_EIGENVALUE. We had to ac- count for boundary SPC constraints as well as beam reference nodes to get the accumulated percentage to add up to 100%. ◦ Fixed a problem reporting redundant constraints for MPP Implicit. ◦ Enhanced *CONTACT_AUTO_MOVE for implicit. ◦ Fixed Implicit handling of *CONSTRAINED_TIE-BREAK in MPP. ◦ Added support for implicit dynamics to *MAT_157 and *MAT_120. ◦ Skip frequency damping during implicit static dynamic relaxation. ◦ Added feature to simulate brake squeal. Transient and mode analysis can be combined to do the brake squeal study by intermittent eigenvalue anal- ysis. *CONTROL_IMPLICIT_ROTATIONAL_DYNAMICS, *CONTROL_IMPLICIT_SOLVER should also be used, setting LCPACK = 3 to enable unsymmetric stiffness matrix. In the non-symmetric stiffness ma- trix analysis such as brake squeal analysis, the damping ratio, defined as - 2.0*RE(eigenvalue)/ABS(IMG(eigenvalue)), can be output to the eigout file and plotted in LS-PrePost. A negative damping ratio indicates an unstable mode. Besides ◦ Add a warning message if the defined rotational speed is not the same as NOMEG in *CONTROL_IMPLICIT_ROTATIONAL_DYNAMICS. ◦ *CONTROL_IMPLICIT: Fixed a bug to initialize velocity correctly when using a displacement file in dynamic relaxation for implicit MPP. ◦ Nonlinear implicit solver 12 is made default implicit solver, which is aimed for enhanced robustness in particular relation to BFGS and line search. ◦ Parameter IACC available on *CONTROL_ACCURACY to invoke en- hanced accuracy in selected elements, materials and tied contacts. Includ- ed is strong objectivity in the most common elements, strong objecitity and physical respons in most commont tied contacts and full iteration plasticity in *MATs 24 and 123. For more detailed information refer to the manual. INTRODUCTION ◦ Bathe composite time integration scheme implemented for increased stabil- ity and conservation of energy/momentum, see *CONTROL_IMPLICIT_ DYNAMICS. Time integration parameter ALPHA on CONTROL_ IMPLICIT_DYNAMICS is used for activation. ◦ For NLNORM.LT.0 all scalar products in implicit are with respect to all degrees of freedom, sum of translational and rotational (similar to NLNORM.EQ.4), the rotational dofs are scaled using ABS(NLNORM) as a characteristic length to appropriately deal with con- sistency of units. that just ◦ The message 'convergence prevented due to unfulfilled bc...' has annoyed users. Here this is loosened up a little and also accompanied with a check that the bc that prevents convergence is actually nonzero. Earlier this pre- vention has activated even for SPCs modelled as prescribed zero motion, which does not make sense. ◦ Implicit now writes out the last converged state to the d3plot database on error termination if not already written. ◦ Fixed bug for *CONTROL_IMPLICIT_MODAL_DYNAMIC if jobid is used. • *INITIAL ◦ Fix incorrect NPLANE and NTHICK for *INITIAL_STRESS_SHELL when output to dynain file for shell type 9. ◦ Fix *INITIAL_STRAIN_SHELL output to dynain for shell types 12 to 15 in 2D analysis. ◦ Write out strain at only 1 intg point if INTSTRN = 0 in *INTERFACE_ SPRINGBACK_LSDYNA and all strains at all 4 intg points if INTSTRN = 1 and nip = 4 in *SECTION_SHELL. ◦ *INITIAL_EOS_ALE: Allow initialization of internal energy density, rela- tive volume, or pressure in ALE elements by part, part set, or element set. ◦ *INITIAL_VOLUME_FRACTION_GEOMETRY: Add option (FAMMG < 0) to form pairs of groups in *SET_MULTI-MATERIAL_GROUP_LIST to re- place the first group of the pair by the second one. ◦ *INITIAL_STRESS_DEPTH can now work with parts that have an Equa- tion of State (EOS types 1, 4, 6 only). Note however that *INITIAL_ STRESS_DEPTH does not work with ALE. ◦ Fix several instances of overwriting the initial velocities of any interface nodes read in from a linking file (SMP only). ◦ *INITIAL_VOLUME_FRACTION_GEOMETRY: Add local coordinate sys- tem option for box. ◦ The initial strain and energy is calculated for *INITIAL_FOAM_ REFERENCE_GEOMETRY. ◦ Add the option of defining the direction cosine using two nodes for *INITIAL_VELOCITY_GENERATION. INTRODUCTION ◦ Fix incorrect transformation of *DEFINE_BOX which results in incorrect initial velocities if the box is used in *INITIAL_VELOCITY. ◦ Fix incorrect initial velocity when using *INITIAL_VELOCITY with NX = - 999. ◦ Fix seg fault when using *INITIAL_INTERNAL_DOF_SOLID_TYPE4 in dynain file. ◦ Do not transform the translational velocities in *INITIAL_VELOCITY or *INITIAL_VELOCITY_GENERATION if the local coordinate system ICID is defined. ◦ Fix uninitialized *INITIAL_VELOCITY_ GENERATION with STYP = 2, i.e. part id, for *ELEMENT_SHELL_ COMPOSITE/*ELEMENT_TSHELL_COMPOSITE. velocities when using ◦ Fix incorrect initialization of velocities if using *INITIAL_VELOCITY_ GENERATION with STYP = 1, i.e. part set for shells with formulation 23 & 24. ◦ Fix incorrect initial velocity and also mass output to d3hsp for shell types 23 & 24. ◦ Fix incorrect initial velocities when using *INITIAL_VELOCITY_ GENERATION with irigid = 1 and *PART_INERTIA with xc = yc = zc = 0 and nodeid > 0 with *DEFINE_TRANSFORMATION. ◦ Fix incorrect stress initialization of *MAT_057/MAT_LOW_DENSITY_ FOAM using dynain file with *INITIAL_STRESS_SOLID when NHISV is equal to the number of history variables for this mat 57. ◦ Fix seg fault when reading dynain.bin ◦ Fixed stress initialization (*INITIAL_STRESS_SECTION) for type 13 tetra- hedral elements. The pressure smoothing was causing incorrect pressure values in the elements adjacent to the prescribed elements. ◦ Assign initial velocities (*INITIAL_VELOCITY) to beam nodes that are generated when release conditions are defined (RT1, RT2, RR1, RR2 on *ELEMENT_BEAM.) ◦ Added an option to retain bending stiffness in spot weld beams that have prescribed axial force. To use is, set KBEND = 1 on *INITIAL_AXIAL_ FORCE_BEAM. ◦ Fix for *INITIAL_STRESS_BEAM when used with spotweld beam type 9. It was possible that error/warning message INI+140 popped up even if number of integration points matched exactly. ◦ Fix for the combination of type 13 tet elements and *INITIAL_STRESS_ SOLID. The necessary nodal values for averaging (element volume, Jaco- bian) were not correctly initialized. Now the initial volume (IVEFLG) is used to compute the correct initial nodal volume. • Isogeometric Elements ◦ Enable spc boundary condition to be applied to extra nodes of nurbs shell, see *CONSTRAINED_NODES_TO_NURBS_SHELL INTRODUCTION ◦ Fix a bug for isogeometric element contact, IGACTC = 1, that happens when more than one NURBS patches are used to model a part so that a in- terpolated elements have nodes belonging to different NURB patches. ◦ *ELEMENT_SOLID_NURBS_PATCH: Enable isogeometric analysis for solid elements, it is now able to do explicit and implicit analysis, such as contact and eigenvalue analysis, etc. Add mode stress analysis for isogeometric solid and shell elements so that the isogeometric element is also able to do frequency domain analysis. ◦ Add reduced, patch-wise integration rule for C1-continuous quadratic NURBS. This can be used by setting INT = 2 in *ELEMENT_SHELL_ NURBS_PATCH. ◦ Add trimmed NURBS capability. Define NL trimming loops to specify a trimmed NURBS patch. Use *DEFINE_CURVE (DATTYP = 6) to specify define trimming edges in the parametric space. ◦ Fix bug in added mass report for *ELEMENT_SHELL_NURBS_PATCH in MPP. • *LOAD ◦ *LOAD_GRAVITY_PART and staged construction (*DEFINE_STAGED_ CONSTRUCTION_PART) were ignoring non-structural mass MAREA (shells) and NSM (beams). Now fixed. ◦ Fix for *INTERFACE_LINKING in MPP when used with adaptivity. ◦ Updates for *INTERFACE_LINKING so that it can be used with adaptiv- ity, provided the linked parts are adapting. ◦ Fix for *INTERFACE_LINKING when used with LSDA based files gener- ated by older versions of the code. ◦ *DEFINE_CURVE_FUNCTION: Functions "DELAY", PIDCTL" and "IF" of are revised. Add sampling rate and saturation limit to PIDCTL of *DEFINE_ CURVE_FUNCTION. "DELAY" of *DEFINE_CURVE_FUNCTION can delay the value of a time-dependent curve by "-TDLY" time steps when TDLY < 0. ◦ Add edge loading option to *LOAD_SEGMENT_SET_NONUNIFORM. ◦ Fix insufficient memory error,SOL+659, when using *LOAD_ERODING_ PART_SET with mpp. ◦ Fix incorrect loading when using *LOAD_ERODING_PART_SET with BOXID defined. INTRODUCTION ◦ Fix incorrect pressure applied if the directional cosines, V1/V2/V3, for *LOAD_SEGMENT_SET_NONUNIFORM do not correspond to a unit vec- tor. ◦ Add *DEFINE_FUNCTION capability to *LOAD_SEGMENT_SET for 2D analysis. ◦ Fix incorrect behavior when using arrival time, AT, or box, BOXID, in *LOAD_ERODING_PART_SET. ◦ Fix error when runing analysis with *LOAD_THERMAL_CONSTANT_ ELEMENT_(OPTION) in MPP with ncpu > 1. ◦ Fixed *LOAD_STEADY_STATE_ROLLING when used with shell form 2 when used with Belytschko-Wong-Chang warping stiffness (BWC = 1 *CONTROL_SHELL). ◦ Add "TIMESTEP" as a code defined value available for *DEFINE_ FUNCTION and *DEFINE_CURVE_FUNCTION. It holds the current simulation timestep. ◦ Fixed issues involving *LOAD_THERMAL_D3PLOT. ◦ Allow extraction of node numbers in loadsetud for all values of LTYPE in *USER_LOADING_SET. Comments included appropriately in the code. Argument list of loadsetud is changed accordingly. ◦ Implemented SPF simulation (*LOAD_SUPERPLASTIC_FORMING) for 2d problems. ◦ Added effective stress as target variable for SPF simulation. ◦ Added box option for SPF simulation to limit target search regions. • *MAT ◦ Fix output to d3hsp for *MAT_HYPERELASTIC_RUBBER. Broken in r93028. ◦ Error terminate with message, KEY+1115, if_STOCHASTIC option is in- voked for *MATs 10,15,24,81,98, 123 but no *DEFINE_STOCHASTIC_ VARIATION or *DEFINE_HAZ_PROPERTIES keyword is present in the input file. ◦ Fix spurious error termination when using *DEFINE_HAZ_PROPERTIES with adaptivity. ◦ Fixed *MATs 161 and 162 when run with MPP. The array that is used to share delamination data across processors had errors. ◦ *MAT_261/*MAT_262: Fixed problem using *DAMPING_PART_ STIFFNESS together with RYLEN = 2 in *CONTROL_ENERGY. ◦ Added safety check for martensite phase kinetics in *MAT_244. ◦ Fix for combination of *MAT_024_STOCHASTIC and shell elementstype 13, 14, and 15 (with 3d stress state). ◦ Fix bug in *MATs 21 and 23 when used with *MAT_ADD_THERMAL_ EXPANSION. ◦ *MAT_ALE_VISCOUS: Implement a user defined routine in dyn21.F to compute the dynamic viscosity. INTRODUCTION ◦ Add histlist.txt to usermat package. This file lists the history variables by material. ◦ Bug in *MAT_089 fixed: The load curve LCSS specifies the relationship be- tween "maximum equivalent strain" and the von Mises stress. The "maxi- mum equivalent strain" includes both elastic and plastic components. The material model was not calculating this variable as intended, so was not following LCSS accurately. The error was likely to be more noticeable when elastic strains are a significant proportion of the total strain e.g. for small strains or low initial Youngs modulus. ◦ Fixed bug affecting *MAT_119: unpredictable unloading behaviour in local T-direction if there are curves only for the T-direction and not for the S- direction. ◦ Fixed bug in *MAT_172: Occured when ELFORM = 1 (Hughes-Liu shell formulation) was combined with Invariant Numbering (INN > 0 on *CONTROL_ACCURACY). In this case, the strain-softening in tension did not work: after cracking, the tensile strength remained constant. ◦ New option for *MAT_079: Load curve LCD defining hysteresis damping versus maximum strain to date. This overrides the default Masing behav- iour. ◦ *MAT_172: Added error termination if user inputs an illegal value for TYPEC. Previously, this condition could lead to abnormal terminations that were difficult to diagnose. Fixed bug affecting ELFORM = 16 shells made of *MAT_172 – spuri- ous strains could develop transverse to the crack opening direction. ◦ Fixed bug in *MAT_ARUP_ADHESIVE (*MAT_169). The displacement to failure in tension was not as implied by the inputs TENMAX and GCTEN. For typical structural adhesives with elastic stiffness of the order of 1000- 10000 MPa, the error was very small. The error became large for lower stiffness materials. ◦ *MAT_SPR_JLR: Modify output variables from *MAT_SPR_JLR . Fix bug that caused spurious results or unexpected element deletion if TELAS = 1. ◦ Fixed bug in *MAT_174 - the code could crash when input parameters EUR = 0 and FRACR = 0.. ◦ Fix MPP problem when writing out aea_crack file for *MAT_WINFRITH. ◦ Include *MAT_196 as one that triggers spot weld thinning. ◦ *MAT_ADD_FATIGUE: Implemented multi slope SN curves to be used in (*FREQUENCY_DOMAIN_RANDOM_ vibration random fatigue INTRODUCTION VIBRATION_FATIGUE) and SSD fatigue (FREQUENCY_DOMAIN_SSD_ FATIGUE). ◦ Guard against possible numerical round off that in some cases might result in unexpected airflow in *MAT_ADD_PORE_AIR. ◦ Added new material *MAT_115_O/*MAT_UNIFIED_CREEP_ORTHO. ◦ *MAT_274: Added support for 2D-solids. New flag (parameter 8 on card 2) is used to switch normal with in-plane axis. ◦ *MAT_255: Fixed bug in plasticity algorithm and changed from total strain rate to plastic strain rate for stability. Added VP option (parameter 5 on card 2) for backwards compatibility: VP = 0 invokes total strain rate used as before. ◦ Added new cohesive material *MAT_279/*MAT_COHESIVE_PAPER to be used in conjunction with *MAT_274/*MAT_PAPER. ◦ User materials: Added support for EOS with user materials for tshell for- mulations 3 and 5. ◦ Fixed bug in dyna.str when using EOS together with shells and orthotropic materials. ◦ *MAT_122: A new version of *MAT_HILL_3R_3D is available. It supports temperature dependent curves for the Young's/shear moduli, Possion ra- tios, and Hill's anisotropy parameters. It also supports 2D-tables of yield curves for different temperatures. Implicit dynamics is supported. The old version is run if parameter 5 on card 3 is set to 1.0. ◦ Added the phase change option to *MAT_216, *MAT_217, *MAT_218 to allow material properties to change as a function of location. This capabil- ity is designed to model materials that change their properties due to ma- terial processing that is otherwise not modeled. For example, increasing the mass and thickness due to the deposition of material by spraying. It is not used for modeling phase changes caused by pressure, thermal loading, or other mechanical processes modeled within LS-DYNA. ◦ Fix internal energy computation of *MAT_ELASTIC_VISCOPLASTIC_ THERMAL/MAT_106. ◦ Fix incorrect results or seg fault for *MAT_FU_CHANG_FOAM/MAT_083 if KCON > 0.0 and TBID.ne.0. ◦ If SIGY = 0 and S = 0 in *MAT_DAMAGE_2/MAT_105, set S = EPS1/200, where EPS1 is the first point of yield stress input or the first ordinate point of the LCSS curve. ◦ Set xt = 1.0E+16 as default if user inputs 0.0 for *MAT_ENHANCED_ COMPOSITE_DAMAGE/MAT_054. Otherwise, random failure of ele- ments may occur. Implemented for thick shells and solids. ◦ Allow *MAT_ENHANCED_COMPOSITE_DAMAGE/MAT_054 failure mechanism to work together with *MAT_ADD_EROSION for shells. ◦ Fix incorrect erosion behavior if *MAT_ADD_EROSION is used with fail- *MAT_123/MAT_MODIFIED_PIECEWISE_ for ure criteria defined LINEAR_PLASTICITY. INTRODUCTION ◦ Fix non-failure of triangular elements type 4 using *MAT_ADD_EROSION with NUMFIP = -100. ◦ Implement scaling of failure strain for *MAT_MODIFIED_PIECEWISE_ for LINEAR_PLASTICITY_STOCHASTIC/MAT_123_STOCHASTIC shells. ◦ Fix incorrect behavior *MAT_LINEAR_ELASTIC_DISCRETE_ BEAM/MAT_066 when using damping with implicit(statics) to explicit switching. for ◦ Fix error due to convergence when using *MAT_CONCRETE_EC2/MAT_ 172 in implicit and when FRACRX = 1.0 or FRACRY = 1.0 ◦ Fix incorrect fitting results for *MAT_OGDEN_RUBBER/MAT_077_O if the number of data points specifed in LCID is > 100. ◦ Fix incorrect fitting results for *MAT_MOONEY-RIVLIN-RUBBER/MAT_ 027 if the number of data points specifed in LCID is > 100. ◦ Fix incorrect forces/moments when preloads are used for *MAT_ 067/NONLINEAR_ELASTIC_DISCRETE_BEAM and the strains changes sign. ◦ Implement *MAT_188/MAT_THERMO_ELASTO_VISCOPLASTIC_ CREEP for 2D implicit analysis. ◦ Support implicit for *MAT_121/MAT_GENERAL_NONLINEAR_1DOF_ DISCRETE_BEAM. ◦ Fix seg fault when using *DEFINE_HAZ_TAILOR_WELDED_BLANK with *DEFINE_HAZ_PROPERTIES. ◦ Fix ineffective *MAT_ADD_EROSION if the MID is defined using a alpha- numeric label. ◦ Fix seg fault when using THERMAL/MAT_255 for solids. *MAT_PIECEWISE_LINEAR_PLASTIC_ ◦ Zero the pressure for *MAT_JOHNSON_HOLMQUIST_JH1/MAT_241 af- ter it completely fractures, i.e. D>=1.0, under tensile load. ◦ Fix incorrect element failure when using EPSTHIN and VP = 0 for *MAT_ 123/MODIFIED_PIECEWISE_LINEAR_PLASTICITY. ◦ Fix error termination when using adaptive remeshing for 2D analysis with *MAT_015/JOHNSON_COOK and NIP = 4 in *SECTION_SHELL and ELFORM = 15. ◦ Fix erosion due to damage, max shear & critical temperature in elastic state for *MAT_MODIFIED_JOHNSON_COOK/MAT_107 for solids. ◦ Check diagonal elements {OPTION}TROPIC_ELASTIC and STR+1306, if any of them are negative. of C-matrix error *MAT_002/MAT_ terminate with message, of ◦ Fix plastic strain tensor update for *MAT_082/*MAT_PLASTICITY_ WITH_DAMAGE. ◦ Fix error when using *MAT_144/MAT_PITZER_CRUSHABLE_FOAM with solid tetahedron type 10. ◦ Fix out-of-range forces after dynamic relaxation when using VP = 1 for *MAT_PIECEWISE_LINEAR_PLASTICITY and non-zero strain rate pa- INTRODUCTION rameters, C & P, and the part goes into plastic deformation during dynam- ic relaxation. ◦ Fixed unit transformation for GAMAB1 and GAMAB2 on *MAT_DRY_ FABRIC. We were incorrectly transforming them as stress. ◦ Fixed implicit solutions with shell elements that use *MAT_040 and lami- nated shell theory. ◦ Fixed the stress calculation in the thermal version of *MAT_077. ◦ Corrected the AOPT = 0 option of ortho/anisotropic materials when use with skewed solid elements. Previously, the material direction was initial- ized to be equivalent to the local coordinate system direction. This is not consistent with the manual for skewed elements which states that the ma- terial a-axis is in the 1-2 directions for AOPT = 0. This is now fixed and the manual is correct. ◦ Fixed the AOPT = 0 option of ortho/anisotropic materials for tetrahedral element forms 10, 13, and 44. ◦ Fixed *MAT_082 for solid elements. An error in the history data was caus- ing possible energy growth or loss of partially damaged elements. ◦ Modified *MAT_FABRIC/*MAT_034 FORM = 24 so that Poisson's effects occur in tension only. ◦ Modified *MAT_221/*MAT_ORTHOTROPIC_SIMPLIFIED_DAMAGE to correct the damage behavior. Prior to this fix, damage was applied to new increments of stress, but not the stress history, so material softening was not possible. ◦ Fixed *MAT_106 when used with curves to define the Young's modulus and Poisson's ratio and when used with thick shell form 5 or 6. The as- sumed strain field was unreasonable which caused implicit convergence to fail. ◦ Added 2 new erosion criteria for *MAT_221/*MAT_ORTHOTROPC_ SIMPLIFIED_DAMAGE. The new options are NERODE = 10: a or b di- rections failure (tensile or compressive) plus out of plane failure bc or ca. NERODE = 11: a or b directions failure (tensile only) plus out of plane failure bc or ca. ◦ Added a new option for shell *MAT_022/*MAT_COMPOSITE_DAMAGE. When ATRACK = 1, the material directions will follow not only element rotation, but also deformation. This option is useful for modeling layered composites, that have material a-directions that vary by layer, by allowing each layer to rotate independently of the others. Within each layer, the b- direction is always orthogonal to the a-direction. ◦ Fixed the TRUE_T option on *MAT_100 and *MAT_100_DA. If the weld connects shells with different thickness and therefore different bending stiffness, the scheme used by TRUE_T to reduce the calculated moment could behave somewhat unpredictably. With the fix, TRUE_T behaves much better, both for single brick welds and brick assemblies. INTRODUCTION ◦ Added a warning message and automatically switch DMGOPT > 0 to DMGOPT = 0 on *MAT_FABRIC when RS < EFAIL or RS = EFAIL. This prevents a problem where weld assemblies did not fail at all when RS = 0. ◦ *MATs 9, 10, 11, 15, 88, and 224 are now available for thick shells, however only *MATs 15, 88, and 224 are available for the 2D tshell forms 1,2, and 6. ◦ Added thick shell support for the STOCHASTIC option of *MATs 10, 15, 24, 81, and 98. ◦ Added support for *MAT_096 for several solid element types including ELFORMs 3, 4, 15, 18, and 23. ◦ Added a MIDFAIL keyword option for *MAT_024, (MAT_PIECEWISE_ LINEAR_PLASTICITY). With this option, element failure does not occur until the failure strain is reached in the mid plane layer. If an even number of layers is used, then the failure occurs when the 2 closest points reach the failure strain. ◦ Enabled *MATs 26 and 126 (HONEYCOMB) to be used with thick shell forms 3, 5, and 7. These was initialized incorrectly causing a zero stress. ◦ Enabled *MAD_ADD_EROSION to be used with beams that have user de- fined integration. Memory allocation was fixed to prevent memory errors. ◦ Enabled OPT = -1 on *MAT_SPOTWELD for solid elements. ◦ Enabled thick shells to use *MATs 103 and 104 in an implicit solution. These materials were lacking some data initialization so they would not converge. ◦ Enabled solid elements with user-defined orthotropic materials to work with the INTOUT and NODOUT options on *DATABASE_EXTENT_ BINARY. The transformation matrix was stored in the wrong place caus- ing strain and stress transformations to fail. ◦ Enabled *MAT_017 to run with thick shell forms 3 and 5. Neither element was initialized correctly to run materials with equations of state. ◦ Add degradation factors and strain rate dependent strength possibility for *MAT_054/*MAT_ENHANCED_COMPOSITE_DAMAGE solids. ◦ Fixed bug in *MAT_058/*MAT_LAMINATED_COMPOSITE_FABRIC when used with strain-rate dependent tables for stiffnesses EA, EB and GAB and LAMSHT = 3. ◦ Add strain rate dependency of ERODS in *MAT_058. ◦ Add possibility to use *DEFINE_FUNCTION for *MAT_SPOTWELD_ DAMAGE_FAILURE (*MAT_100), OPT = -1/0. If FVAL = FunctionID, then a *DEFINE_FUNCTION expression is used to determine the weld failure criterion using the following arguments: func (N_rr, N_rs, N_rt, M_ rr, M_ss, M_tt). ◦ Store tangential and normal separation (delta_II & delta_I) as history vari- ables 1&2 of *MAT_138/*MAT_COHESIVE_MIXED_MODE. ◦ Add second normalized traction-separation load curve (TSLC2) for Mode II in *MAT_186/*MAT_COHESIVE_GENERAL. INTRODUCTION ◦ Fixed bug in using *MAT_157/*MAT_ANISOTROPIC_ELASTIC_ PLASTIC with IHIS.gt.0 for shells. Thickness strain update d3 was not cor- rect and plasticity algorithm failed due to typo. ◦ Fixed bug in *MAT_157 for solids: This affected the correct stress trans- in *DATABASE_ formation for post-processing using CMPFLG = 1 EXTENT_BINARY. ◦ Fixed bug in *MAT_225 (*MAT_VISCOPLASTIC_MIXED_HARDENING) when using Table-Definition together with kinematic hardening. ◦ Add load curves for rate dependent strengths (XC, XT, YC, YT, SC) in *MAT_261/*MAT_LAMINATED_FRACTURE_DAIMLER_PINHO (shells only). ◦ Add table definition for LCSS for rate dependency in *MAT_261 (shells on- ly). ◦ Add load curves for rate dependent strengths (XC, XCO, XT, XTO, YC, YT, *MAT_262/*MAT_LAMINATED_FRACTURE_DAIMLER_ SC) CAMANHO (shells only). in ◦ Fixed bug when using *MAT_261 or *MAT_262 solids (ELFORM = 2). ◦ Add load curves for SIGY and ETAN for rate dependency of *MAT_262 (shells only) ◦ *MAT_021_OPTION Fixed a bug for defining different orientation angles through the thickness of TSHELL elements (formulations 2 and 3) Added new option CURING: Two additional cards are read to define parameters for curing kinet- ics. Formulation is based on Kamal's model and considers one ODE for the state of cure. State of cure does not affect the mechanical parameters of the materi- al. CTE's for othotropic thermal expansione can be defined in a table with respect to state of cure and temperature. An orthotropic chemical shrinkage is accounted for. ◦ *MAT_REINFORCED_THERMOPLASTICS_OPTION (*MAT_249_ OPTION): Fiber shear locking can be defined wrt to the fiber angle or shear an- gle. Output of fiber angle to history variables. Simplified input: Instead of always reading 8 lines, now the user only has to specify data for NFIB fibers. Added fiber elongation to history variables in *MAT_249 for pospro- cessing. New Option UDFIBER (based on a user defined material by BMW): INTRODUCTION • Transversely isotropic hyperelastic formulation for each fi- ber family . • Anisotropic bending behavior based on modified transverse shear stiffnesses. • Best suited for dry NCF's. ◦ *MAT_GENERALIZED_PHASE_CHANGE (*MAT_254): New material that is a generalized version of *MAT_244 with appli- cation to a wider range of metals. Up to 24 different phases can be included. Between each of the phases, the phase transformation can be defined based on a list of generic transformation laws. For heating JMAK and Oddy are implemented. For cooling Koistinen-Marburger, JMAK and Kirkaldy can be chosen. Constant parameters for the transformations are given as 2d tables, parameters depending on temperature (rate) or phase concentration employ 3d tables. Plasticity model (temperature and strain rate dependent) similar to MAT_244. Transformation induced strains. TRIP algorithm included. Temperature dependent mixture rules. Parameter 'dTmax' that defines the maximum temperature increment within a cycle. If the temperature difference at a certain integration point is too high, local subcycling is performed. Implemented for explicit/implicit analysis and for 2d/3d solid ele- ments. ◦ *MAT_ADHESIVE_CURING_VISCOELASTIC (*MAT_277): New material implementation including a temperature dependent curing process of epoxy resin based on the Kamal-Sourour-model. Material formulation is based on *MAT_GENERAL_VISCOELASTIC. Viscoelastic properties defined by the Prony series, coefficients as functions of state of cure. Chemical and thermal shrinkage considered (differential or secant formulations). Available for shell and solid elements. Can be used in combination with *MAT_ADD_COHESIVE. Implemented for explicit and implicit analysis. An incremental and a total stress calculation procedure available. ◦ Enable *MAT_ADD_EROSION to be safely used with material models that have more than 69 history variables, for now the new limit is 119. INTRODUCTION ◦ Use correct element ID for output of failed solid elements when GISSMO (*MAT_ADD_EROSION) is used with *CONTROL_DEBUG. ◦ Improve performance of GISSMO (*MAT_ADD_EROSION with ID- AM = 1), especially when used with *MAT_024, no other failure criteria, shell elements, and DMGEXP = 1 or 2. Allows speed-up of 10 to 20 per- cent. ◦ Add new keyword *MAT_ADD_GENERALIZED_DAMAGE. It provides a very flexible approach to add non-isotropic (tensorial) damage to stand- ard materials in a modular fashion. Solely works with shell elements at the moment. ◦ Correct the computation of effective strain for options ERODS < 0 in *MAT_058 (*MAT_LAMINATED_COMPOSITE_FABRIC) and EFS < 0 in *MAT_261 (*MAT_LAMINATED_FRACTURE_ DAIMLER_...). The shear strain term was twice the size as it should have been. *MAT_262 and ◦ Adjust stiffness for time step calculation in *MAT_076 and subsequent models (*MAT_176, *MAT_276, ...) to prevent rarely observed instabilities. ◦ Add output of original and fitted curves to messag and separate file (curveplot_<MID>) for *MAT_103. ◦ In *MAT_104 (*MAT_DAMAGE_1), stress-strain curve LCSS can now be used directly with all FLAG options (-1,0,1,10,11), no fitting. ◦ Correct strain calculation for anisotropic damage in *MAT_104 (*MAT_ DAMAGE_1) with FLAG = -1. ◦ Initialize stress triaxiality of *MAT_107 (*MAT_MODIFIED_JOHNSON_ COOK) to zero instead of 1/3. ◦ Avoid negative damage in *MAT_107 (*MAT_MODIFIED_JOHNSON_ COOK) with FLAG2 = 0 for solid elements. ◦ Rectify the characteristic element length in *MAT_138 (*MAT_COHESIVE_ MIXED_MODE) for solids type 21 and 22 (cohesive pentas) and shell type 29 (cohesive shell) for "curve" options T < 0 and S < 0. ◦ Correct/improve material tangent for *MAT_181 with PR > 0 (foam op- tion). ◦ Add possibility to define logarithmically defined strain rate table LCID-T in material *MAT_187 (*MAT_SAMP-1). ◦ Fix missing offset when using *DEFINE_TRANSFORMATION with load curve LCID-P in *MAT_187 (*MAT_SAMP-1). ◦ Add reasonable limit for biaxial strength in *MAT_187 with RBCFAC > 0.5 to avoid concave yield surface. ◦ Improve performance of *MAT_187 to reach speed-up of 10 to 40 percent, depending on which options are used. ◦ Add new option for *MAT_224 (*MAT_TABULATED_JOHNSON_COOK). With BETA < 0 not only a load curve but now also a table can be referred to. The table contains strain rate dependent curves, each for a different temperature. INTRODUCTION ◦ Fix for implicit version of *MAT_224 (*MAT_TABULATED_JOHNSON_ COOK). Computations with shell elements should converge faster now. ◦ *MAT_224 (*MAT_TABULATED_JOHNSON_COOK) can now be used in implicit even with temperature dependent Young's modulus (parameter E < 0). ◦ Always store the Lode parameter as history variable #10 in *MAT_224 (*MAT_TABULATED_JOHNSON_COOK), not just for LCF being a table. ◦ Variable LCI of *MAT_224 / *MAT_224_GYS can now refer to a *DEFINE_ TABLE_3D. That means the plastic failure strain can now be a function of Lode parameter (TABLE_3D), triaxiality (TABLE), and element size (CURVE). ◦ For thick shells type 1 and 2, the element size in *MAT_224 is now correct. ◦ Add new option for definition of parameters FG1 and FG2 in *MAT_240 (*MAT_COHESIVE_MIXED_MODE_ELASTOPLASTIC_RATE). ◦ Add new option to *MAT_240: new load curves LCGIC and LCGIIC define fracture energies GIC and GIIC as functions of cohesive element thickness. GIC_0, GIC_INF, GIIC_0, and GIIC_INF are ignored in that case. ◦ Add new feature to *MAT_248 (*MAT_PHS_BMW). Estimated Hocket- Sherby parameters are written to history variables based on input func- tions and phase fractions. ◦ Add new option ISLC = 2 to *MAT_248 (*MAT_PHS_BMW) which allows to define load curves (cooling rate dependent values) for QR2, QR3, QR4, and all parameters on Cards 10 and 11. ◦ Add new option LCSS to *MAT_252 (*MAT_TOUGHENED_ADHESIVE_ POLYMER): A load curve, table or 3d table can now be used to define rate and temperature dependent stress-strain behavior (yield curve). ◦ Fix for *MAT_255, evaluation of 2d tables LCIDC and LCDIT. Negative temperatures were interpreted as logarithmic rates. ◦ Add new material model *MAT_280 (*MAT_GLASS) for shell elements. It is a smeared fixed crack model with a selection of different brittle, stress- state dependent failure criteria and crack closure effects. ◦ *DEFINE_FABRIC_ASSEMBLIES: Assemblies of *MAT_FABRIC part sets can be specified to properly treat bending of t-intersecting fabrics that are stitched or sewn together. See ECOAT, TCOAT and SCOAT on *MAT_ FABRIC_... Bending can only occur within an assembly, aka a part set. ◦ *MAT_USER_DEFINED_MATERIAL_MODELS: In user defined material models, a logical parameter 'reject' can be set to .true. to indicate to the implicit solver that equilibrium iterations should be aborted. The criterion is the choise of the implementor, but it could be if plastic strain increases by more than say 5% in one step or damage increases too much, whatever that might render an inaccurate prediction and bad results. Setting this pa- rameter for explicit won't do anything. ◦ IHYPER = 3 for user shell materials now supports thickness train update, see *MAT_USER_DEFINED_MATERIAL_MODELS. INTRODUCTION ◦ *MAT_SIMPLIFIED_RUBBER/FOAM: AVGOPT < 0 is now supported for the FOAM option, which activates a time averaged strain rate scheme to avoid noisy response. ◦ MAT_181 is now supported for 2D implicit simulations. ◦ *MAT_ADD_EROSION: A number of extensions and improvements to the DIEM damage model were made, IDAM < 0. General efficiency, it was slow, now it's GOT to be faster. NCS can be used as a plastic strain increment to only evaluate criteria in quantifications of plastic strain. NUMFIP < 0 is employing the GISSMO approach, number of layers for erosion. A new ductile damage criterion based on principal stress added (DMITYP = 4). MSFLD and FLD can be evaluated in mid or outer layers to separate membrane and bending instability (P2). MSFLD and FLD can use an incremental or direct update of instabil- ity parameter (P3). Output of integration point failure information made optional (Q2). Specifying DCTYP = -1 on the damage evolution card will not couple damage to stress but the damage variable is only calculated and stored. ◦ *MAT_SMOOTH_VISCOELASTIC_VISCOPLASTIC, *MAT_275: An elas- tic-plastic model with smooth transition between elastic and plastic mode is available. It incorporates viscoelasticity and viscoplasticity and is based on hyper-elastoplasticity so it is valid for arbitrarily large deformations and rotations. A sophisticated parameter estimation is required to match test data, it is available for implicit and explicit analyisis but perhaps most- ly suited for implicit. ◦ *MAT_FABRIC_MAP: Stress map material 34 is equipped with bending properties identical to that of the form 14 and form -14 version of the fab- ric. Coating properties are set in terms of stiffness, thickness and yield. The material is supported in implicit, including optional accounting for the nonsymmetric tangent. Should be used with bending stiffness on, and convergence is improved dramatically if geometric stiffness is turned on. ◦ *MAT_084 with predefined units (CONM < 0) is now transformed correct- ly with INCLUDE_TRANSFORM. ◦ If LCIDTE = 0 in *MAT_121, then LS-DYNA was crashing on some plat- forms, including Windows. This is fixed. ◦ Fix initialization issues so that PML models can be run with *CASE com- mands. ◦ *MAT_027 is revised to avoid accuracy issues for single precision executa- bles. INTRODUCTION ◦ The nearly imcompressible condition is enhanced for *MAT_027 shell ele- ments. ◦ Add a new material model as a option for *MAT_165. *MAT_PLASTIC_ NONLINEAR_KINEMATIC_B is a mixed hardening material model, and can be used for fatigue analysis. ◦ Output local z-stress in *MAT_037, when *LOAD_STRESS_SURFACE is used. This was previously calculated and saved as another history varia- ble. ◦ Add a new material model *MAT_260 (2 forms). Uses non-associated flow rule and Hill's yield surface; including strain rate effect and temperate effect. MIT failure criteria is also im- plemented. Implemented for solids and shells. Strain rate sensitivity for solids. Option to directly input the Pij and Gij values. Separate the material model *MAT_260 into *MAT_260A and *MAT_ 260B: • MAT260A=*MAT_STOUGHTON_NON_ASSOCIATED_ FLOW • MAT260B=*MAT_MOHR_NON_ASSOCIATED_FLOW Incorporates FLD into the fracture strain, so as to consider the mesh size effect. Calculates the characteristic length of the element for *MAT_260B, so that an size-dependent failure criterial can be used. When failure happens for half of the integration points through the thickness, the element is deleted. ◦ Add Formablitiy Index to *MAT_036, *MAT_037, *MAT_226. ◦ Add new history variables for Formability Index, affecting *MAT_036, *MAT_037, *MAT_125, *MAT_226. Those new history variables are FI, be- ta, effective strain. These comes after the 4 regular history variables. ◦ *MAT_036, *MAT_125: New option_NLP is added to evaluate formability under non-linear strain paths. User inputs a forming limit diagram (FLD), and Formablitiy Index (F.I.) will be automatically converted to effective stain vs. beta based space. • MPP ◦ Fix problem of MPP pre-decomposition that can occur if the local directory specified in the pfile has very different lengths in the initial run vs the ac- tual run The difference resulted in a line count difference in the size of the structured files created, throwing off the reading of the file in the actual run. ◦ Straighten out some silist/sidist issues in MPP decomp: INTRODUCTION silist and sidist outside of a "region" in the pfile are no longer sup- ported, and an error message is issued which suggests the use of "re- gion { silist" instead. They have been undocumented for several years (since "region" was introduced), and had other issues. ◦ Fix the keywords, CONTROL_MPP_DECOMPOSITION_CONTACT_ and CONTROL_MPP_DECOMPOSITION_CONTACT_ DISTRIBUTE ISOLATE, which were not treating each contact interface individually (as the manual states), but collectively. ◦ Fix for MPP decomp of part sets. ◦ Fixed *CONTROL_MPP_PFILE (when used inside an include file) so that it honors ID offsets from *INCLUDE_TRANSFORM for parts, part sets, and contact ids referenced in "decomp { region {" specifications. Furthermore, such a region can contain a "local" designation, in which case the decom- position of that region will be done in the coordinate system local to the in- clude file, not the global system. For example: *CONTROL_MPP_PFILE decomp { region {partset 12 local c2r 30 0 -30 0 1 0 1 0 0}} would apply the c2r transformation in the coordinate system of the include file, which wasn't previously possible. The local option can be useful even if there are no such transformations, as the "cubes" the decomposition uses will be oriented in the coordinate system of the include file, not the global system. Furthermore, the following decomposition related keywords now have a_LOCAL option, which has the same effect: *CONTROL_MPP_DECOMPOSITION_PARTS_DISTRIBUTE_ LOCAL *CONTROL_MPP_DECOMPOSITION_PARTSET_DISTRIBUTE_ LOCAL *CONTROL_MPP_DECOMPOSITION_ARRANGE_PARTS_LOCAL *CONTROL_MPP_DECOMPOSITION_CONTACT_DISTRIBUTE_ LOCAL ◦ Revert revision 86884, which was: "MPP: change to the decomposition behavior of *CONTROL_MPP_ DECOMPOSITION_PARTS_DISTRIBUTE *CONTROL_MPP_DECOMPOSITION_PARTSET_DISTRIBUTE *CONTROL_MPP_DECOMPOSITION_ARRANGE_PARTS in the case where a decomposition transformation is also used. Previ- ously, any such regions were distributed without the transformation being applied. This has been fixed so that any given transformation applies to these regions also. So now the transformations will NOT INTRODUCTION apply to these keywords. Really, the "region" syntax should be used together with *CONTROL_MPP_PFILE as it is more specific. ◦ Modify behavior of DECOMPOSITION_AUTOMATIC so that if the initial velocity used is subject to *INCLUDE_TRANSFORM, the transformed ve- locities are used. ◦ Fix MPP decomposition issue with "decomp { automatic }" which was not honored when in the pfile. ◦ Save hex weld creation orientation to the pre-decomposition file so that the subsequent run generates the welds in the same way. ◦ Fix for MPP not handling element deletion properly in some cases at de- composition boundaries. ◦ Add new pfile option "contact { keep_acnodes }" which does NOT exclude slave nodes of adaptive constraints from contact, which is the default be- havior. (MPP only.) ◦ MPP Performance-Related Improvements: Allow user input of *LOAD_SEGMENT_FILE through familied files. Bug fix for *LOAD_SEGMENT_FILE to get correct time history data for pressure interpolation. Output two csv files for user to check MPP performance: • load_profile.csv: general load balance • cont_profile.csv: contact load balance Allow user to control decomp/distribution of multiple airbags using *CONTROL_MPP_DECOMPOSITION_ARRANGE_PARTS memory2 = option on *KEYWORD line Disable unreferenced curves after decomposition using *CONTROL_ MPP_DECOMPOSITION_DISABLE_UNREF_CURVES. This applies to the curves used in the following options to speed up the execution several times. • • • • *BOUNDARY_PRESCRIBED_MOTION_NODE *LOAD_NODE *LOAD_SHELL_ELEMENT *LOAD_THERMAL_VARIABLE_NODE ◦ Bug fix for *CONTROL_MPP_DECOMPOSITION_SHOW with *AIRBAG_ PARTICLE. ◦ Fix cpu dependent results when using function RCFORC() in *DEFINE_ CURVE_FUNCTION. This affects MPP only. ◦ Fix hang up when using *DEFINE_CURVE_FUNCTION with element function BEAM(id,jflag,comp,rm) and running MPP with np > 1. ◦ *CONTROL_MPP_DECOMPOSITION: The cpu cost for solid elements -1 and -2 are accounted for in the mpp domain decomposition. ◦ Fix bug in *CONTROL_MPP_IO (Windows platform only) related to insuf- ficient administrative privileges for writing tmp file on root drive. ◦ Revise l2a utility on Windows platform to create identical node output INTRODUCTION format as Linux. • Output ◦ Fix for MPP external work when bndout is output and there are *BOUNDARY_PRESCRIBED_MOTION_RIGID commands in the input. ◦ Fixed the output of forces and associated energy due to *LOAD_RIGID_ BODY for both explicit and implicit (*DATABASE_BNDOUT). ◦ Fixed stress and strain output of thick shells when the composite material flag is set on *DATABASE_EXTENT_BINARY. The transformation was backwards. ◦ If the size of a single plot state was larger than the d3plot size defined by x=<factor> on the execution line, the d3plot database may not be readable by LS-PrePost. This issue is now fixed. ◦ *DATABASE_PROFILE: Output data profiles for beams (TYPE = 5) and add density as DATA = 20. ◦ New option HYDRO = 4 on *DATABASE_EXTENT_BINARY. Outputs 7 additional variables: the same 5 as HYDRO = 2 plus volumetric strain (de- fined as Relative Volume - 1.0) and hourglass energy per unit initial vol- ume. ◦ Fix for binout output of swforc file which can get the data vs. ids out of sync when some solid spotwelds fail. ◦ Fix for d3plot output of very large data sets in single precision. ◦ Fix for output of bndout data for joints in MPP, which was writing out in- correct data in some cases. ◦ Added new option *INTERFACE_SPRINGBACK_EXCLUDE to exclude selected portions from the generated dynain file. ◦ Add a new option to *INTERFACE_COMPONENT_FILE to output only 3 degrees of freedom to the file, even if the current model has 6. ◦ Minor change to how pressure is computed for triangles in the INTFOR output. ◦ Fix MPP output issue with intfor file. ◦ Fixes for writing and reading of dynain data in LSDA format. ◦ Corrected the summation of rigid body moments for output to bndout for some special cases in MPP. ◦ Corrected the output to d3iter when 10 node tets are present (D3ITCTL on *CONTROL_IMPLICIT_SOLUTION). ◦ Enhanced implicit collection of moments for the rcforc file. ◦ For implicit, convert spc constraint resultant forces to local coordinate sys- tem for output. Also corrected Implicit's gathering of resultant forces due to certain SPC constraints. ◦ Fixed the gathering of resultant forces in implicit for prescribed motion on nodes of a constrained rigid body for output to bndout. INTRODUCTION ◦ Added output of modal dynamics modal variables to a new file moddy- is controlled by *CONTROL_IMPLICIT_MODAL_ Output nout. DYNAMICS. ◦ Corrected the output of resultant forces for Implicit Linear analysis. Cor- rected the output of resultant forces for MPP executions. These enhance- ments affect a number of ASCII files including bndout. ◦ The following 4 enhancements are to the eigensolvers, including that used for *CONTROL_IMPLICIT_EIGENVALUE. Standardized and enhance the warning/error messages for Implicit eigensolution for the case where zero eigenmodes are computed and returned in eigout and d3eigv. Added nonsymmetric terms to the stiffness matrix for the implicit ro- tational dynamics eigenanalysis. This allows brake squeal analysis with the contact nonsymmetric terms from mortar contact now in- cluded in the analysis. Updated implicit eigensolution for problems with unsymmetric stiff- ness matrices. Fixed Rotational Dynamics eigensolution to work cor- rectly when first order matrix (W) is null. . Added the eigensolution for problems with stiffess (symmetric or un- symmetric), mass, and damping. ◦ Improve Implicit's treatment of constrained joints to account for rounding to *CONSTRAINED_JOINT with *CONTROL_ Applicable errors. IMPLICIT_GENERAL. ◦ For implicit springback, zero out the forces being reported to rcforc for those contact interfaces disabled at the time of springback. Also enhance the removal of contact interfaces for springback computations. For *INTERFACE_SPRINGBACK. ◦ *DATABASE_RECOVER_NODE is available to recover nodal stress. ◦ Fix a bug for detailed stress output, eloutdet, for SOLID type 18. ◦ Support new format of interface force files for ALE, DEM, and CPM. LS- PrePost can display the correct label for each output component. ◦ Added *DATABASE_NCFORC_FILTER option to allow the NCFORC data to be filtered using either single pass or double pass Butterworth filtering to smooth the output. Added the same filtering capability to *DATABASE_BINARY_D3PLOT. This capability is specified on the addi- tional card for the D3PLOT option and does not require "_FILTER" in the keyword input. ◦ Fix incorrect mass properties for solids in SSSTAT file when using *DATABASE_SSSTAT_MASS_PROPERTIES. ◦ Fix seg fault during writing of dynain file if INSTRN = 1 in *INTERFACE_ SPRINGBACK and STRFLG.ne.0 in *DATABASE_EXTENT_BINARY and the SPRINGBACK. Also output warning message, KEY+1104. comes after *INTERFACE_ ◦ Fix zero strain values output to curvout for *DEFINE_CURVE_ FUNCTION using function, ELHIST, for solid elements. ◦ Fix missing parts in d3part when MSSCL = 1 or 2 in *DATABASE_ EXTENT_BINARY. ◦ Fix incorrect damping energy computation for glstat. ◦ Fix incorrect part mass in d3plot for shells, beams & thick shells. ◦ Fix incorrect curvout values when using BEAM(id,jflag,comp,rm) for *DEFINE_CURVE_FUNCTION and if the beam formulation is type 3, i.e. truss. ◦ Fix incorrect output to curvout file if using ELHIST in *DEFINE_CURVE_ FUNCTION for shells. ◦ Output stresses for all 4 intg points to eloutdet for cohesive element types 19 & 20. ◦ Fix incorrect rotational displacement to nodout when REF = 2 in *DATABASE_HISTORY_NODE_LOCAL. Affects MPP only. ◦ Fix incorrect strains output to elout for shell type 5 and when NIP > 1. ◦ Fix incorrect acceleration output to nodout file when IACCOP = 1 in *ELEMENT_SEATBELT_ IGRAV = 1 in *CONTROL_OUTPUT and ACCELEROMETER. ◦ Fix corrupted d3plot when RESPLT = 1 in *DATABASE_EXTENT_ BINARY and idrflg.ge.5 in *CONTROL_DYNAMIC_RELAXATION. ◦ Fix missing element connectivities in nastin file when using *INTERFACE_ SPRINGBACK_NASTRAN_NOTHICKNESS. fault when using seg ◦ Fix *DATABASE_BINARY_D3PART with *CONTACT_TIED_SHELL_EDGE_TO_SURFACE. This affects SMP only. ◦ Fix incorrect output to bndout when using multiple *LOAD_NODE_ POINT for the same node and running MPP with ncpu > 1. ◦ Fix incorrect dyna.inc file when using *MAT_FU_CHANG_FOAM/MAT_ 83, *DEFINE_COORDINATE_NODES, and *CONSTRAINED_JOINT_ STIFFNESS_GENERALIZED with *INCLUDE_TRANSFORM. ◦ Fix IEVERP in *DATABASE_EXTENT_D3PART which was not honored in writing out d3part files. ◦ Fix incorrect stresses written out to dynain for thick shells with formula- tions 1,2 and 4. ◦ Fix incorrect output to disbout data for discrete beams. ◦ Fix incorrect output to binary format of disbout. Affects SMP only. ◦ Fix error when writing initial stresses for thick shells to dynain. Affects MPP only. ◦ Fix thick shells strain output to dynain. ◦ Fix incorrect writing of material data to dyna.str for *MAT_SEATBELT when using long = s. ◦ Fix coordinate/disp output to d3plot of *CONSTRAINED_NODAL_ RIGID_BODY's pnode. INTRODUCTION ◦ Fixed the initial d3plot state in SMP runs when tied contact is used with theCNTCO parameter on *CONTROL_SHELL. The geometry was wrong in that state. ◦ Add cross section forces output (*DATABASE_SECFORC) for cohesive el- ements ELFORM type 19, 20, 21, and 22. ◦ Slight increase of precision for values in nodout file. ◦ Add new option FSPLIT to *INTERFACE_SPRINGBACK_LSDYNA to split the dynain file into two files (geometry and initial values). ◦ *DEFINE_MATERIAL_HISTORIES: New keyword for organizing material history outputs, currently only for solids, shells and beams and the d3plot output but to be extended to tshells and ascii/binout. The purpose is to customize that otherwise are output via NEIPS/NEIPH/NEIPB on *DATABASE_EXTENT_BINARY, to avoid vari- able conflict and large d3plots and thus facilitate post-processing of these variables. Currently available in small scale but to be continuously ex- tended. the history variables ◦ Fixed bug affecting IBINARY = 1 (32 bit ieee format) in *DATABASE_ FORMAT. This option was not working. ◦ Fixed incorrect printout of node ID for *ELEMENT_INERTIA. ◦ Increased the header length to 80 for the following files in binout: matsum, nodout, spcforc, ncforc ◦ Fixed bug in which d3msg was not written for SMP. ◦ The d3plot output for rigid surface contact was incorrect for MPP. ◦ Fixed bugs when when using curve LCDT to control d3plot output. ◦ Fixed abnormal increase in d3plot size caused by outputting velocity and acceleration when data compression is on. ◦ Added new variable GEOM in *CONTROL_OUTPUT for chosing geome- try or displacement in d3plot, d3part, and d3drlf. ◦ Added command line option "msg=" to output warning/error descrip- tions. See MSGFLG in *CONTROL_OUTPUT for alternate method of re- questing such output. Accepted values for "msg=" are message# or all. message#, e.g., KEY+101 or 10101. This option will print the er- ror/warning message to the screen. all. this option will print all error/warning messages to d3msg file. ◦ Fixed bug for *DATABASE_BINARY_D3PROP file if adaptivity used. The error caused blank d3prop output. ◦ *DATABASE_HISTORY_SHELL_SET *CONTROL_ ADAPTIVITY caused error 20211. The error involves the BOX option be- ing used for shell history output. combined with ◦ Added *INTEGRATION... data to d3prop. INTRODUCTION • Restarts ◦ Fix bug when deleted uniform pressure (UP) airbag during simple restart. ◦ Fix for index error that could cause problems for accelerometers during full deck restart in MPP. ◦ Fix for MPP output of LSDA interface linking file when restarting from a dump file. ◦ Fix incorrect strains in d3plot after restart when STRLG > 1. ◦ Fix incorrect velocity initialization for SMP full deck restart when using ◦ *INITIAL_VELOCITY_GENERATION *INITIAL_VELOCITY_ and GENERATION_START_TIME. ◦ Fix incorrect behavior of *CONTACT_ENTITY in full deck restart. ◦ Fix incorrect full deck restart analysis if initial run was implicit and the full deck restart run is explicit. ◦ Fix ineffective boundary condition for *MAT_RIGID when using *CHANGE_RIGID_BODY_CONSTRAINT with *RIGID_DEFORMABLE_ R2D for small deck restart. ◦ Fix initialization of velocities of *MAT_RIGID_DISCRETE nodes after re- start using *CHANGE_VELOCITY_GENERATION. ◦ Fix internal energy oscillation after full deck restart when using *CONTACT_TIED_SURFACE_TO_SURFACE_OFFSET with TIEDID = 1 in optional card D. This affects SMP only. ◦ Corrected bug affecting full restart that included any change to node/element IDs. This bug has existed since version R6. ◦ Fixed bug affecting d3plot times following fulldeck restart with curve in SMP. ◦ Fixed bug in simple restart: *INTERFACE_COMPONENT_FILE forgets the filename and writes to infmak instead. • *SENSOR ◦ Enable full restart for *SENSOR. ◦ Add optional filter ID to SENSORD of *DEFINE_CURVE_FUNCTION. ◦ Enable LOCAL option of *CONSTRAINED_JOINT to be used with *SENSOR_DEFINE_FORCE. ◦ Fix a MPP bug that happens when *SENSOR_DEFINE_NODE has a de- fined N2. ◦ *SENSOR_CONTROL: Fix a bug for TYPE = JOINTSTIF Fix a MPP bug for TYPE = PRESC-MOT when the node subject to prescribed motion is part of a rigid body Add TYPE = BELTSLIP to control the lockup of *ELEMENT_ SEATBELT_SLIPRING. Add TYPE = DISC-ELES to delete a set of discrete elements. INTRODUCTION ◦ Add FTYPE = CONTACT2D to to *SENSOR_DEFINE_FORCE to track the force from *CONTACT_2D. ◦ Add the variable SETOPT for *SENSOR_DEFINE_NODE_SET and *SENSOR_DEFINE_ELEMENT_SET to sense and process data from a node set or element set, resp., resulting in a single reported value. ◦ *SENSOR can be used to control *CONTACT_GUIDED_CABLE. ◦ Fix a bug related to *SENSOR_DEFINE_FUNCTION triggered by more than 10 sensor definitions. • SPG (Smooth Particle Galerkin) ◦ *SECTION_SOLID_SPG (KERNEL = 1): The dilation parameters (DX,DY,DZ) of SPG Eulerian kernel are automatically adjusted according to the local material deformation to prevent tensile instability. • SPH (Smooth Particle Hydrodynamics) ◦ Retain user IDs of SPH particles in order to ensure consistent results when changing the order of include files. ◦ Add feature to inject SPH particles, *DEFINE_SPH_INJECTION. ◦ Added support of various material models for 2D and 3D SPH particles: *MAT_098 (*MAT_SIMPLIFIED_JOHNSON_COOK) *MAT_181 (*MAT_SIMPLIFIED_RUBBER) *MAT_275 (*MAT_SMOOTH_VISCOELASTIC_VISCOPLASTIC) ◦ Added support of *DEFINE_ADAPTIVE_SOLID_TO_SPH for 2D shell el- ements and 2D axisymmetric shell elements. ◦ When using *DEFINE_ADAPTIVE_SOLID_TO_SPH, eliminated duplicate kinetic energy calculation for SPH hybrid elements (both SPH particles and solid elements contributed kinetic energy into global kinetic energy). ◦ Added support of second order stress update (OSU = 1 in *CONTROL_ ACCURACY keyword) for 2D and 3D SPH particles. This is necessary for simulation of spinning parts. ◦ Added ISYMP option in *CONTROL_SPH to define as a percentage of original SPH particles the amount of memory allocated for generation of SPH ghost nodes used in *BOUNDARY_SPH_SYMMETRY_PLANE. ◦ Fixed unsupported part and part set option in *BOUNDARY_SPH_FLOW. ◦ Fixed unsupported ICONT option from *CONTROL_SPH when combined with *BOUNDARY_SPH_FLOW. ◦ *DEFINE_SPH_TO_SPH_COUPLING: Output contact forces between two SPH parts (x,y,z and resultant forces) into sphout. The forces can be plotted by LS-PrePost. ◦ *CONTACT_2D_NODE_TO_SOLID: Added bucket sort searching algo- rithm to speed up the process of finding contact pairs between SPH parti- cles and solid segments. INTRODUCTION • Thermal ◦ Corrected a long standing bug in MPP thermal associated with spotwelds (*CONSTRAINED_SPOTWELD) using thermal linear solver option 11 or greater. The spotweld loads were not being loaded correctly due to an in- dexing issue in MPP. ◦ Fix for thermal with *CASE. ◦ Fix MPP support for thermal friction in SOFT = 4 contact. ◦ Fixed bug where thermal solver gives a non-zero residual even though no loads are present. ◦ Added SOLVER = 17 (GMRES solver) to *CONTROL_THERMAL_ SOLVER for the conjugate heat transfer problem. The GMRES solver has been developed as an alternative to the direct solvers in cases where the structural thermal problem is coupled with the fluid thermal problem in a monolithic approach using the ICFD solver. A significant savings of calcu- lation time can be observed when the problem reaches 1M elements. This solver is implemented for both SMP and MPP. ◦ *CONTACT_(option)_THERMAL (3D contact only): Add variable FRTOHT to specify fraction of frictional energy applied to slave surface. It follows that 1.-FRTOHT is applied to master surface. Default is 0.5 which gives a 50% - 50% split between the slave and master surfaces which was hardwired in prior releases. ◦ First release of AUTOMATIC_SURFACE_TO_SURFACE_TIED_WELD_ THERMAL. This will only work when used with BOUNDARY_ THERMAL_WELD. This combination of keywords will activate a condi- tion where sliding contact will become tied contact on cooldown when the temperature of the segments in contact go above an input specified tem- perature limit during welding. ◦ *LOAD_THERMAL_D3PLOT: The d3plot data base was changed such that the 1st family member contains control words, geometry, and other control entities. Time state data begins in the 2nd family member. This change al- lows the new d3plot data structure to be read in by LS-DYNA when using the *LOAD_THERMAL_D3PLOT keyword. This change is not backward compatible. The old d3plot data structure will no longer be read correctly by LS-DYNA. ◦ Synchronize data in TPRINT for SMP and MPP: Fixed output to tprint/binout for thermal contact. Fixed part IDs for part energies. Fixed format of TPRINT file generated by l2a. ◦ Fixed handling of start time defined with *CONTROL_START for thermal solver. ◦ Change the maximum number of *LOAD_HEAT_CONTROLLER defini- tions from 10 to 20. INTRODUCTION ◦ Added a third parameter to the TIED_WELD contact option. The parame- ter specifies heat transfer coefficient h_contweld for the welded contact. Before welding, the parameter from the standard card of the thermal con- tact is used. ◦ Parameter FRCENG supported for mortar contact to yield heat in coupled thermomechanical problems. • XFEM (eXtended Finite Element Method) ◦ Added ductile failure to XFEM using critical effective plastic strain as fail- ure criterion. • Miscellaneous ◦ Support *SET_NODE_GENERAL PART with SPH and DES. ◦ *DEFINE_POROUS_...: Compute the coefficients A and B with a user de- fined routine in dyn21.F. bugs ◦ Fixed in Staged Construction (*DEFINE_STAGED_ CONSTRUCTION_PART): Staged construction not working on SMP parallel. Symptoms could include wrong elements being deleted. Staged construction with beam elements of ELFORM = 2: when these beams are dormant, they could still control the time step. Staged construction with *PART_COMPOSITE. The bug occurred when different material types were used for different layers within the same part, and that part becomes active during the analysis. The symptom of the bug was that stresses and/or history variables were not set to zero when the part becomes active. ◦ Bugs fixed in *DAMPING_FREQUENCY_RANGE_DEFORM: Incorrect results when large rigid body rotations occur. If RYLEN on *CONTROL_ENERGY = 2, the energy associated with this damping should be included in the Internal Energy for the rele- vant part(s). This energy was being calculated only if there was also *DAMPING_PART_STIFFNESS in the model. Now fixed - the damp- ing energy will be included in the internal energy whenever RYLEN = 2. ◦ Fixed NID option of *DEFINE_COORDINATE_VECTOR (bug occurred in MPP only). ◦ Fix lsda open mode to require only minimal permissions to avoid unneces- sary errors, for example if using an interface linking file that is read only. ◦ Fix for DPART processing (*SET_..._GENERAL) for solid and thick shell elements. INTRODUCTION ◦ Fix for JOBID > 63 characters. ◦ Fix input processing problem (hang) that could happen in some unusual cases if encrypted *INCLUDE files are used. ◦ Fix interaction of *CASE with jobid = on command line, so the jobid on the command line is combined with the generated case ids instead of being ig- nored. ◦ *INCLUDE_NASTRAN: Integration defaults to Lobatto for Nastran translator. The default number of integration points is set to 5 for Nastran trans- lator. ◦ Issue error message TRANSFORMATION is specified. and terminate when illegal *DEFINE_ ◦ Add OPTION = POS6N to *DEFINE_TRANSFORMATION to define trans- formation with 3 reference nodes and 3 target nodes. ◦ Add OPTION = MIRROR to *DEFINE_TRANSFORMATION. ◦ Fix a bug that could occur when adapted elements are defined in a file in- cluded by *INCLUDE_TRANSFORM. ◦ Fix a bug that could occur when *BOUNDARY_SPC_SYMMETRIC_ PLANE is used together with *INCLUDE_TRANSFORM. ◦ Fix a bug that occurs when *DEFINE_BOX is included by *INCLUDE_ TRANSFORM. ◦ Make *SET_NODE_COLLECT work together with *NODE_SET_MERGE. ◦ Fix incorrect shell set generated when using *SET_SHELL_GENERAL with OPTION = PART. ◦ Add error trap for *SET_PART_LIST_GENERATE_COLLECT to catch missing part IDs. ◦ Fixed bug in *INCLUDE_TRANSFORM for adaptive case if JOBID is used. ◦ Fixed bug in memory allocation for *DEFINE_CURVE if total number of points in curve is more than 100. ◦ Fixed bug with *INCLUDE_TRANSFORM and *CONTROL_ADAPTIVITY due to an *INCLUDE inside *INCLUDE_TRANSFORM file. Added new The *NODE, files: adapt.inc# *ELEMENT_SHELL and *ELEMENT_SOLID are removed from include file. for *INCLUDE_TRANSFORM file. ◦ Fixed bug for DPART option in *SET_SEGMENT_GENERAL. DPART op- tion was treated as PART option before. ◦ Fixed failure of *PARAMETER definition in long format. ◦ Fixed error in reading solid id for *SET_SOLID_GENERAL. ◦ Ignore any nonexistant part set IDs in *SET_PART_ADD. ◦ Fix bug in which sense switches sw2 and sw4 don't work when the output interval for glstat is small. ◦ Fixed bug if *DEFINE_CURVE is used to define adaptivity level. INTRODUCTION ◦ Three new keywords are implemented in support of user defined subrou- tines: *MODULE_PATH[_RELATIVE], MODULE_LOAD, MODULE_USE. The MODULE feature allows users to compile user subroutines into dynamic libraries without linking to the LS-DYNA main executable. The dynamic libraries are independent from the main executable and do not need to be recompiled or linked if the main executable is up- dated. This feature loads multiple dynamic libraries on demand as specified in the keywords. Without the MODULE feature, only one version of each umat (such as umat41) can be implemented. With the MODULE feature, most umat subroutines can be have multiple versions in multiple dynamic libraries, and used simultaneously. The MODULE feature supports all user subroutines. The LS-DYNA main executable may also run without any dynamic libraries if no user subroutines are required. Capabilities added to create LS-DYNA R10.0: See release notes (published separately) for further details. • *AIRBAG ◦ Enhance the robustness of *AIRBAG_INTERACTION to help avoid insta- bility in MPP when the interaction involves more than two bags. ◦ *AIRBAG_PARTICLE: Adjust dm_out calculation of vent hole to avoid truncation error. Fix bug in chamber output when there are multiple airbags and mul- tiple chambers not in sequential order. Bug fix for closed volume of airbag/chamber with intersecting tubes. Add new feature to allow user to define local coordinates of jetting of particles through internal vents. Support *SENSOR_CONTROL for CPM airbag. CPM is not supported for dynamic relaxation. Disable CPM airbag feature during DR and reactivate airbag following DR. Allow solid parts in definition of internal part set. The solid volume will be excluded from the airbag volume. Allow additional internal part set for shells. The shell part should form a closed volume and its volume will be excluded from the air- bag volume. • *ALE INTRODUCTION ◦ *LOAD_BLAST_SEGMENT: Automatically generate the ALE ambient el- ements attached to a segment or segment set. ◦ *BOUNDARY_AMBIENT_EOS: implement *DEFINE_CURVE_FUNCTION for the internal energy and relative vol- ume curves. ◦ *CONTROL_ALE, *CONSTRAINED_LAGRANGE_IN_SOLID and *ALE_REFERENCE_SYSTEM: If NBKT < 0 in *CONTROL_ALE, call *DEFINE_CURVE to load a curve defining the number of cycles between bucket sorting in function of time. If NBKT > 0, the bucket sorting is acti- vated if the mesh rotations and deformations are large. ◦ *ALE_FSI_TO_LOAD_NODE: Implement a mapping of the FSI accelera- tions by forces/masses) *CONSTRAINED_LAGRANGE_IN_SOLID (ctype = 4) between different meshes. computed (penalty ◦ DATABASE_FSI, and *DATABASE_BINARY_FSILNK: Add a parameter CID to output fsi forces in a local coordinate system. ◦ Structured ALE (S-ALE) solver: *DATABASE_BINARY_FSIFOR ALE models using rectilinear mesh can be directly converted to S- ALE models and run using S-ALE solver by assigning CPIDX = -1 in *ALE_STRUCTURED_MESH. S-ALE via *ALE_STRUCTURED_MESH_CONTROL_POINTS. progressive mesh generation RATIO in ◦ Recode ALE Donor Cell/Van Leer advection routines and restructure communication algorithm. *CONSTRAINED_LAGRANGE_IN_SOLID These give 30% improvement in run time. • *BOUNDARY ◦ *BOUNDARY_PWP can now accept a *DEFINE_FUNCTION instead of a load curve. The input arguments are the same as for *LOAD_SEGMENT: (time, x, y, z, x0, y0, z0). option for of *BOUNDARY_PRESCRIBED_ORIENTATION_RIGID to offset the curves by the birth time. "toffset" ◦ Add ◦ MPP now supports MCOL coupling, *BOUNDARY_MCOL. ◦ Fix bug of there being fully constrained motion of a rigid part when pre- with one in scribing translational *BOUNDARY_PRESCRIBED_MOTION_RIGID while *MAT_RIGID, i.e., all rotational dof are constrained. dof con2 = 7 more than ◦ Instead of error terminating with warning message, STR+1371, when *BOUNDARY_PRESCRIBED_MOTION and *BOUNDARY_SPC is applied INTRODUCTION to same node and dof, issue warning message, KEY+1106, and release the conflicting SPC. erroneous SET_BOX results option used for is if ◦ Fix *BOUNDARY_PRESCRIBED_MOTION. ◦ Fix *BOUNDARY_PRESCRIBED_ACCELEROMETER_RIGID for MPP. It may error terminate or give wrong results if more than one of this key- word is used. ◦ Fix segmentation using *BOUNDARY_PRESCRIBED_ORIENTATION with vad = 2, i.e. cubic spline interpolation. when fault ◦ Added instruction *BOUNDARY_ACOUSTIC_IMPEDANCE for explicit calculations that applies an impedance boundary condition to the bounda- ry of *MAT_ACOUSTIC element faces. This is a generalization of the non- and reflecting *BOUNDARY_ACOUSTIC_IMPEDANCE may be used on the same faces, in which case the boundary acts like both and entrant and exit boundary. ◦ Fixed a problem with non-reflecting boundaries redefining the bulk modu- condition. boundary *LOAD Both lus which caused contact to change behavior. ◦ Added support for acoustic materials ith non-reflective boundaries. ◦ Fix the single precision version so that *INCLUDE_UNITCELL now has no problem to identify pairs of nodes in periodic boundaries. ◦ When using *INCLUDE_UNITCELL to generate Periodic Boundary Con- straints (PBC) for an existing mesh, a new include file with PBCs is gener- ated instead of changing the original mesh input file. For example, if users include a file named "mesh.k" through *INCLUDE_UNITCELL (INPT = 0), a new include file named "uc_mesh.k" is generated where all PBCs are de- fined automatically following the original model information in mesh.k. ◦ *INCLUDE_UNITCELL now supports long input format in defining the element IDs. ◦ Include SPC boundary conditions as part of H8TOH20 solid element con- version. ◦ Add a new option SET_LINE to *BOUNDARY_PRESCRIBED_MOTION: This option allows a node set to be generated including existing nodes and new nodes created from h-adaptive mesh refinement along the straight line connecting two specified nodes to be included in prescribed boundary conditions. • BLAST ◦ *PARTICLE_BLAST and DES: Consider eroding of shell and solid in particle_blast. Support interface force file output for gas particle-structure coupling. Bug fix for wet DES coupled with beam. Support *SET_NODE_GENERAL PART with SPH or DES. INTRODUCTION MPP now uses async communication for DES coupling to improve general performance. Support for solid element when modeling irregular shaped charge with HECTYPE = 0/1 in *PARTICLE_BLAST. Output adaptive generated DES and NODE to a keyword file. ◦ Fix inadvertent detonation of HE part when there are more than one HE is not defined with the HE part though even part and *INITIAL_DETONATION. explicit to explicit ◦ Fixed *BOUNDARY_USA_COUPLING support *INITIAL_STRESS and *INITIAL_STRAIN_ usage, typically from a dynain file. ◦ Fixed support *CONTROL_DYNAMIC_RELAXATION IDRFLF = 5, so a static implicit calculation can be used to initialize/preload a model before conducting an explicit transient calculation. If inertia relief is used during the static phase, with *CONTROL_IMPLICIT_INERTIA_RELIEF for the explilcit phase. *BOUNDARY_USA_COUPLING disabled must then be to it ◦ Support imperial unit system for *PARTICLE_BLAST. mass = lbf-s2/in, length = inch, time = second, force = lbf, pressure = psi. ◦ Add option to define detonation point using a node for *PARTICLE_BLAST. ◦ Add interface force file output for *PARTICLE_BLAST with keyword *DATABASE_BINARY_PBMFOR and command line option "pbm=". This output of forces for gas-particle-structure coupling. ◦ For *PARTICLE_BLAST, add built-in smoothing function for particle struc- ture interaction. ◦ For *PARTICLE_BLAST, when coupling with DEM, the DEM nodes that are inside HE domain are automatically deactivated. ◦ Add support for solid elements when modeling irregular shaped charge with HECTYPE = 0/1 for *PARTICLE_BLAST. The original approach only supports shell elements and the initial coordinates of HE particle are at shell surface. The model had to relax several hundred time step to let par- ticle fill in the interior space, which was not convenient. Using new ap- proach, the initial positions of HE particles are randomly distributed inside the container by using solid element geometry. Both hex and Tet solids are supported. ◦ For particle blast method (PBM), consider reflecting plane as infinite. ◦ Change the name of keyword *DEFINE_PBLAST_GEOMETRY to *DEFINE_PBLAST_HEGEO. • *CESE (Compressible Fluid Solver) ◦ CESE time steps: INTRODUCTION Modified the blast wave boundary condition treatment to make it (with calculations stable wave more blast *LOAD_BLAST_ENHANCED). in The flow field calculation will be skipped if the structural time-step is much smaller than the fluid time step, until both time-steps reach the same order. This will save CPU time in some fluid/structure interac- tion (FSI) problem calculations. In addition to depending upon the local CFL number, the fluid time step 'dt' calculation has been modified to also adjust dynamically to extreme flow conditions. This makes stiff flow problems more stable especially in 3D fluid problem calculations when the mesh quality is poor. ◦ Moving mesh solvers: Corrected several aspects of the implicit ball-vertex (BV) mesh mo- tion solver for the following keywords: *ICFD_CONTROL_MESH_MOV *CESE_CONTROL_MESH_MOV. The absolute tolerance argument is no longer used by the BV solver. As an example, the following is all that is needed for CESE moving mesh problems: *CESE_CONTROL_MESH_MOV $ ialg numiter reltol 1 500 1.0e-4 Also corrected the CESE moving mesh solvers for a special case in- volving a wedge element. Also, fixed the d3plot output of wedge el- ement connectivities for the CESE moving mesh solvers. ◦ CESE d3plot output: Added real 2D CESE output, and this is confirmed to work with LSPP4.3 and later versions. This also works for d3plot output with the 2D CESE axisymmetric solver. For all immersed-boundary CESE solvers, corrected the plotting of the Schlieren number and the chemical species mass fractions. The following new CESE input cards are related to surface d3plot output: *CESE_SURFACE_MECHSSID_D3PLOT *CESE_SURFACE_MECHVARS_D3PLOT In conjunction with the above, new FSI and conjugate heat transfer output on solid (volume) mesh outside boundaries is now supported. ◦ CESE immersed-boundary method (IBM) FSI solvers: INTRODUCTION *CESE_FSI_EXCLUDE is a new keyword for use with the CESE im- mersed boundary method FSI solvers. With it, unnecessary structur- al parts that are not actively participating in the FSI in the CESE IBM- FSI solver can now be excluded from the CESE FSI calculation. This is also supported for the case when some of the mechanics parts in- volve element erosion. ◦ CESE chemistry solvers: In R10, we also updated several things in the FSI solver with chemis- try called FSIC. In chemical reacting flow, a delta time between itera- tions is extremely important for code stabilization and thus, to get reasonable results. To this end, we optimized such an iterative delta time, which is based on the CFL number. This optimization is based on the gradient of the local pressure, which we think will dominate control of the CFL number. Next, the total number of species are increased up to 60 species in chemical reacting flow, so that the reduced Ethylene (24~53 species) and Methane (20~60 species) combustion are possible with this ver- sion. We will update more practical examples about FSIC problems includ- ing precise experimental validations. Note that we can provide some related examples upon user request. Other corrections of note include the following: Brought in enthalpy-related corrections to the CESE chemistry solv- ers. Fixed the conjugate heat transfer boundary condition for the 2D and 3D CESE fixed mesh chemistry solvers. Corrected the initialization of fluid pressure for CESE IBM chemistry solvers. Enabled output of the timing information for the CESE chemistry solvers. Added restart capability to the CESE chemistry solvers. • *CHEMISTRY ◦ New inflator models of Pyrotechnic and Hybrid type are updated. It is important to note that these are basically 0-dimensional models via the fol- lowing two main keywords, *CHEMISTRY CONTROL_INFLATOR *CHEMISTRY_INFLATOR_PROPERTIES ◦ By using the *CHEMISTRY CONTROL_INFLATOR keyword, the user can select the type of the solver, output mode, running time, delta t, and time interval for output of time history data. For example, if we have a keyword set up as, INTRODUCTION *CHEMISTRY CONTROL_INFLATOR, $ isolver ioutput runtime delt p_time 1 0 0.1 1.0e-6 5.0e-4 with "isolver set to 1", the user can simulate a conventional Pyrotechnic in- flator mode, while with "isolver" set to 2 or 3, Hybrid inflator simulation is possible. ◦ In addition, to continue an airbag simulation via an ALE or CPM method, the user can save the corresponding input data file by using "ioutput" op- tion. For more details about airbag simulations using a saved data file, re- fer to the keyword manual. ◦ Also, note that the updated version has two options for the Hybrid models: isolver = 2 => Hybrid model for the cold flow isolver = 3 => Hybrid model for the heated flow. ◦ In the *CHEMISTRY_INFLATOR_PROPERTIES keyword, there are sever- al cards to set up the required properties of an inflator model. The first two cards are for the propellant properties involved in inflator combustion. For example, $card1: propellants $ comp_id p_dia p_height p_mass p_tmass 10 0.003 0.0013 2.0e-5 5.425e-3 $card2: control parameters $ t_flame pindex A0 trise rconst 2473. 0.4 4.45e-5 0.0 0.037 In the first card, the user can specify the total amount of propellant parti- cles and their shape. Using the second card, the user can also specify the thermodynamics of the propellant and its burning rate. To support the options in card2, especially the second option, pindex, and the third, A0, we provide a standalone program upon request for the pro- pellant equilibrium simulation. The remaining cards are for the combustion chamber, gas chamber, and airbag, respectively. • *CONTACT ◦ *CONTACT_AUTOMATIC_SURFACE_TO_SURFACE_MORTAR_TIED_ WELD for modeling welding has been added. Surfaces are tied based on meeting temperature and proximity criteria. Non-MORTAR version of this contact was introduced at R9.0.1. ◦ Fix issue setting contact thickness for rigid shells in ERODING contact. ◦ Add MPP support for *CONTACT_AUTOMATIC_GENERAL with adap- tivity. INTRODUCTION ◦ Change "Interface Pressure" report in intfor file from abs (force/area) to - force/area, which gives the proper sign in case of a tied interface in ten- sion. ◦ Rework input processing so that more than one *CONTACT_INTERIOR may be used, and there can be multiple part sets in each one. ◦ Minor change to how pressure is computed for triangles in the intfor data- base. ◦ Fix 2 bugs for contact involving high order shell elements: - When high order shell elements are generated by SHL4_TO_SHL8. - When using a large part id like 100000001. ◦ Implement a split-pinball based contact option for neighbor elements in segment-based contact. Invoke this option by setting |SFNBR|>=1000. The new algorithm is more compatible with DEPTH = 45 so that there is no longer a need to split quads. ◦ The effect of shell reference system offsets on contact surface location is now properly considered when running MPP. The shell offset may be specified using NLOC in *SECTION_SHELL or in *PART_COMPOSITE, or by using the OFFSET option of *ELEMENT_SHELL. This effect on contact is only considered when CNTCO is set to 1 or 2 in *CONTROL_SHELL. ◦ Fix of bug for *CONTACT_AUTOMATIC_SURFACE_TO_SURFACE after dynamic re- laxation when consistency is on in SMP. time = 0.0 forces rcforc zero in at ◦ Fix input error when using many *RIGIDWALL_GEOMETRIC_... with _DISPLAY option. ◦ Fix input error when *CONTACT_ENTITY is attached to a beam part, PID. ◦ Fix error termination due to negative volume, SOL+509, even when *CONTACT_ERODING... is set. This affects MPP only. ◦ Check whether a slave/master node belongs to a shell before updating the nodal *CONTROL_SHELL and SST/MST.ne.0.0 and in SSFT/SMFT = 0.0 card 3 of *CONTACT_..... For SMP only. thickness when ISTUPD > 0.0 in ◦ Fix penetrating nodes when ◦ Fix *CONTACT_ERODING_NODES_TO_SURFACE with *MAT_142/*MAT_ seg using *CONTACT_AUTOMATIC_SINGLE_SURFACE_TIED with consistency mode, .i.e. ncpu < 0, for SMP. when fault SOFT = 1 using in ◦ Fix corrupted intfor when using parts/part sets in *CONTACT_AUTOMATIC_....This affects SMP only. ◦ Implement incremental update of normal option, invoked by TIEDID = 1, for *CONTACT_TIED_NODES_TO_SURFACE_CONSTRAINED_OFFSET for SMP. ◦ Fix unconstrained nodes when using *CONTACT_TIED_SURFACE_TO_SURFACE_CONSTRAINED_OFFSET resulting in warning message, SOL+540. This affects SMP only. INTRODUCTION ◦ Fix spurious repositioning of nodes when using *CONTACT_SURFACE_TO_SURFACE for SMP. ◦ Added support to segment based contact for the SRNDE parameter on op- tional card E. This option allows round edge extensions that do not extend beyond shell edges and also square edges. The latter overlaps with the SHLEDG parameter on card D. ◦ Fixed a potential memory error that could occur during segment based contact input. ◦ Fixed an error that could cause an MPP job to hang in phase 3. The error could occur when SOFT = 2 contact is used with the periodic intersection check and process 0 does not participate in the contact. ◦ Modified SOFT = 2 contact friction when used with *PART_CONTACT to define friction coefficients, and the two parts in contact have different coef- ficient values. With this change, the mu values used for contact will be the average of the values that are calculated for each part. Prior to this change, mu was calculated for only the part that is judged to be the master. This change makes the behavior more predictable and also makes it behave like the other contacts with SOFT = 0 and SOFT = 1. ◦ Fixed ◦ Added a warning message (STR+1392) for when trying to use the OR- THO_FRICTION contact option with SOFT = 2 contact, because that option is not available. The contact type is switched to SOFT = 1. in MPP *CONTACT_2D_AUTOMATIC_SURFACE_TO_SURFACE when used with node sets to define the contact surfaces. The master side was likely to trigger a spurious error about missing nodes that terminated the job. serious error file not force could support NFAIL = 1 ◦ Switched segment based (SOFT = 2) non-eroding contact to prevent it from adding any new segments when brick element faces are exposed when other elements are deleted. There were two problems. The first is that the interface on *DATABASE_EXTENT_INTFOR because the intfor file does not expect new segments to replace the old, so it just undeletes the old segments in- stead of adding the new. The second problem is that when non-eroding contact is used, we only have enough memory in fixed length arrays for the segments that exist at t = 0. When segments are deleted, I was using the space that they vacated to create new segments, but it was very likely that some segments could not be created when the number of open spaces was less than the number of new segments that are needed. In this case, some segments would not be created and there would be surfaces that could be penetrated with no resistance. This behavior is impossible to predict, so it seems better to prevent any new segments from being created unless eroding contact is used. ◦ Fixed rcforc output for MPP 2D automatic contact. The forces across pro- cessors were missed. INTRODUCTION ◦ Fixed a segment based contact error in checking airbag segments. This af- fects only airbags that are defined by control volumes, that is defined by *AIRBAG. The symptom was a segmentation fault. ◦ Fixed SMP eroding segment based (SOFT = 2) contact which was not acti- vating the negative volume checking of brick elements. The MPP contact and the other SMP contacts were doing this but not SMP SOFT = 2. ◦ Fixed support for CNTCO on *CONTROL_SHELL by segment based (SOFT = 2) contact. It was adjusting the contact surface only half of what it should have done. ◦ Fixed eroding segment based contact when used with the CNTCO > 0 on *CONTROL_CONTACT. A segmentation fault was occurring. ◦ Modified MPP segment based (soft = 2) contact to use R8 buffers to pass nodal coordinates. This should reduce MPP scatter when decomposition changes. ◦ Added support for using a box to limit the contact segments to those ini- tially in the box when using eroding segment based contact. The box op- tion has not been available for any eroding contact up until now. (SOFT = 2 and SBOXID, MBOXID on *CONTACT_ERODING_...). ◦ Fixed force transducers with MPP segment based contact when segments are involved with multiple, 2-surface force transducers. The symptom was that some forces were missed for contact between segments on different partitions. ◦ Added support for *ELEMENT_SOURCE_SINK used with segment based contact. With this update, inactive elements are no longer checked for con- tact. ◦ Fixed an MPP problem in segment based contact that cased a divide by ze- ro during the bucket sort. During an iteration of the bucket sort, all active segments were somehow in one plane which was far from the origin such that a dimension rounded to zero. The fix for this should affect only this rare case and have no effect on most models. ◦ Modified segment based (SOFT = 2) contact to make SMP and hybrid fast- er, particularly for larger numbers of processors. ◦ Fixed thermal MPP segment based contact. The message passing of ther- mal energy due to friction was being skipped unless peak force data was written to the intfor file. ◦ Fixed likely memory errors in MPP problems with 2D automatic contact when friction is used. ◦ Support the VC parameter (coefficient for viscous friction) in the case of segment based contact, which has previously been unsupported. This op- tion will work best with FNLSCL > 0, DNLSCL = 0 on optional card D. The card D option causes the contact force to be proportional to the over- lap area which causes even pressure distribution. ◦ Enabled segment based contact (SMP and MPP) to work with type 24 (27- node) brick elements. INTRODUCTION ◦ Fixed MPP segment based contact for implicit solutions. During a line search, some data was not restored correctly when the solver goes back to the last converged state. This caused possible memory errors. ◦ Fixed friction for MPP segment based contact in the implicit solver. The sliding velocity was calculated incorrectly using the explicit time step ra- ther than the implicit step. ◦ Fixed a bug in MPP *CONTACT_2D_AUTOMATIC..., where a flaw in code used during MPP initialization could cause segments to fail to detect penetration. ◦ Fixed the of *CONTACT_2D_AUTOMATIC_SINGLE_SURFACE in the MPP version. There was a memory error that could occur if thick beams were in the model. checking beam thick ◦ New values history (*USER_INTERFACE_FRICTION): material directions, relative velocity components and yield stress. element friction user for ◦ Add new user-defined interface for tiebreak contact invoked by *CONTACT_AUTOMATIC_ONE_WAY_SURFACE_TO_SURFACE_TIEB REAK_USER. ◦ MORTAR CONTACT PENMAX and SLDTHK has taken over the meanings of SST and TKSLS in R9 and earlier, although in a different way. Now PENMAX corresponds to the maximum penetration depth for solid elements (if nonzero, otherwise it is a characteristic length). SLDTHK is used to offset the contact surface from the physical surface of the solid ele- ment, instead of playing with SST and TKSLS, which was rather awkward. This update also saves the pain of having to treat shells and solids in separate interfaces if these features are wanted. This changes the behavior in some inputs that did have SST turned on for solids, but a necessary measure to make the contact decent for future versions. The characteristic length for solid elements has been revised to not result in too small sizes that would lead to high contact stiffnesses and less margin for maximum penetration. SFS on CONTACT_..._MORTAR can be input as negative, then con- tact pressure is the -SFS load curve value vs penetration. Smooth roundoffs of sharp edges in MORTAR contact has been ex- tended to high order segments, meaning that edge contact is valid even in this case. The MORTAR contact now honors the NLOC parameter for shells, see *SECTION_SHELL, adjusting the contact geometry accordingly. Note that CNTCO on *CONTROL_SHELL applies as if always active, meaning that if NLOC is on, then CNTCO will also be "on" for MOR- TAR contacts. INTRODUCTION Output of contact gaps to the intfor file is now supported for MOR- TAR contact, see *DATABASE_EXTENT_INTFOR. Transducer contacts, *CONTACT_..._FORCE_TRANSDUCER, are supported for MORTAR contact in SMP and MPP. A disclaimer is that the slave and master sets in the transducer have to be defined through parts or part sets. Warnings are issued if this is violated. Option 2 is now supported for tiebreak MORTAR contact, *CONTACT_..._MORTAR_TIEBREAK, but only for small sliding. Options 4 and 7 are supported in the MORTAR tiebreak contact for any type of sliding. For explicit analysis, the bucket sort frequency for MORTAR contact is 100, but can be changed through parameter BSORT on the CON- TACT_..._MORTAR card or NSBCS on CONTROL_CONTACT. Note that the MPP bucket sort parameter does not apply. This assumes to improve the efficiency of MORTAR explicit contact significantly compared to R9 and earlier versions. Dynamic friction is supported in MORTAR contact for explicit and implicit dynamic analysis. See FD and DC on *CONTACT_... card. Wear calculations are supported for the MORTAR contact. See CONTACT_ADD_WEAR. Triangular shell form 24 is supported with MORTAR forming contact and accounts for high order shape functions. Automatic MORTAR contact now supports contact with end faces of beam elements and not just the lateral surfaces. Mortar contact is available in 2D plane strain and axisymmetric simu- lations, but only for SMP implicit. See CONTACT_2D_...MORTAR. ◦ Wear computed from *CONTACT_ADD_WEAR can optionally be output to dynain on optional card of *INTERFACE_SPRINGBACK_LSDYNA. This will generate *INITIAL_CONTACT_WEAR cards for subsequent wear simulations, and LS-DYNA will apply this wear and modify geome- try accordingly. Restrictions as described in the manual apply. ◦ Improve under *CONTACT_FORMING_ONE_WAY_SURFACE_TO_SURFACE to allow users to define part ID and a node set is automatically generated. SOFT = 6 • *CONSTRAINED ◦ Add frictional energy calculation for constraint-based rigid walls. ◦ *CONSTRAINED_BEAM_IN_SOLID: Works with r-adaptivity now. Can now constrain beams in tshells as well as solids. INTRODUCTION ◦ Fix a bug for *CONSTRAINED_LOCAL that might mistakenly constrain z- translation when RC = 0. ◦ The following options do not support MEMORY = auto properly. The MEMORY = auto option will be turned off in this section and report an er- ror if additional memory allocation is needed. *CONSTRAINED_LINEAR_OPTION *CONSTRAINED_MULTIPLE_GLOBAL ◦ Switched translational joints with stiffness to use double precision storage for the displacement value so that the calculated forces are more accurate. This prevents round-off error that can become significant. ◦ Fixed *CONSTRAINED TIED_NODES_FAILURE when used with MPP single surface segment based contact. Non-physical contact between seg- ments that share tied constraints was being penalized leading to failure of the constraints. ◦ The SPR (*CONSTRAINED_SPR2, *CONSTRAINED_INTERPOLATION_SPOTWELD) now the SPOTDEL option of *CONTROL_CONTACT. That means if shell elements involved in the SPR domain fail, the SPR gets deactivated. support models • *CONTROL ◦ Fix possible error ◦ Fix spurious deletion of elements when using TSMIN.ne.0.0 termination with single precision MPP when PSFAIL.ne.0 in *CONTROL_SOLID and using solid formulation 10/13/44. in *CONTROL_TERMINATION, erode = 1 in *CONTROL_TIMESTEP and initialized implicitly in dynamic relaxation. ◦ Added keyword *CONTROL_ACOUSTIC to calculate the nodal motions of *MAT_ACOUSTIC nodes for use in d3plot and time history files. With- out this option the *MAT_ACOUSTIC mesh propagates pressure but does not deform because it uses a linear Eulerian solution method. The struc- tural response is unaffected by this calculation; it is only for visualization and will roughly double the time spent computing acoustic element re- sponse. ◦ When IACC = 1 on *CONTROL_ACCURACY and for shell type 16/-16 in nonlinear implicit, shell thickness change due to membrane strain when ISTUPD > 0 in *CONTROL_SHELL is now included in the solution process and will render continuity in forces between implicit time steps. The out- put contact forces will reflect the equilibrated state rather than the state prior or after the thickness update. is used ◦ Fix bug when RBSMS in *CONTROL_RIGID, affecting mass scaled solu- in conjunction with *ELEMENT_INERTIA and/or on and tions, *PART_INERTIA, *CONSTRAINED_RIGID_BODIES *CONSTRAINED_EXTRA_NODES. specifically with choices IFLAG of ◦ Tshells added to the subcycling scheme (*CONTROL_SUBCYCLE). INTRODUCTION ◦ Tshells and spotweld beams are supported in selective mass scaling. See IMSCL in *CONTROL_TIMESTEP. ◦ Add a new keyword: *CONTROL_FORMING_SHELL_TO_TSHELL to convert shell elements to tshell elements. If a parent node has SPCs, the same SPC constraints will be applied to the corresponding tshell nodes. If adaptivity is invoked, *BOUNDARY_SPC_SET is automatically updated to include newly generated nodes. Allows the normal of the segment set to be changed. Can offset the generated tshells from the mid-surface of the parent shells. Automatically generate segment sets for the top and bottom surfaces, which can be used for contact. • DISCRETE ELEMENT METHOD ◦ Implement generalized for *DEFINE_DE_TO_SURFACE_COUPLING based on the following article in the journal "Wear": Magnee, A., Generalized law of erosion: application to various alloys and intermetallics, Wear, Vol. 181, 500, 1995. erosion law of ◦ Modify tangential force calculation to get better rigid body rotation behav- ior for *DEFINE_DE_BOND ◦ Support restart feature for DEM interface force file and DATABASE out- put. ◦ Instead of using bulk modulus, use mass and time step to estimate contact stiffness for SPH-DEM coupling. This should be better if DEM material is quite different from SPH material. ◦ Fix *DEFINE_DE_MASSFLOW_PLANE bug if DE injection is defined. ◦ Add CID_RCF to *DEFINE_DE_TO_SURFACE_COUPLING for force out- put in local coordinates to 'demrcf' file. ◦ Update the *DEFINE_DE_BY_PART card so that it matches the capabilities of the *CONTROL_DISCRETE_ELEMENT card. ◦ Add penalty stiffness scale factor, thickness scale factor, birth time and death time to *DEFINE_DE_TO_SURFACE_COUPLING. ◦ Add dynamic coefficient of friction to *CONTROL_DISCRETE_ELEMENT. to ◦ Implement Finnie's wear law and user defined wear model *DEFINE_DE_TO_SURFACE_COUPLING. ◦ Implement user-defined curve for DEM frictional coefficient as function of time. ◦ Implement user-defined curve for contact force calculation for *CONTROL_DISCRETE_ELEMENT. ◦ Fix inconsistent results between *DEFINE_DE_BY_PART and *CONTROL_DISCRETE_ELEMENT. INTRODUCTION • *ELEMENT ◦ Fixed bug affecting output from beam elements ELFORM = 2 when certain uncommon inputs are present. Forces and moments in the output files could be wrongly rotated about the beam axis. This affected the output files only, not the solution inside LS-DYNA. The error could occur under two circumstances: (a) if IST on *SECTION_BEAM is non-zero, the output forces and moments are supposed to be rotated into the beam's principal axis system, but this rotation could be applied to the wrong beam ele- ments; and (b) when no ELFORM = 2 elements have IST, but the model al- the so contains beams with ELFORM = 6 and RRCON = 1 on SECTION_BEAM card, some of the ELFORM = 2 elements can have their output forces and moments rotated by 1 radian. ◦ Fix a bug affecting 2d seatbelt with time-dependent slipring friction. ◦ Fix erroneous 1d seatbelt slipring message. ◦ Fix seatbelt consistency issue in SMP (ncpu < 0). ◦ Add error message when 2d seatbelt part doesn't have shell formulation of 5 and *MAT_SEATBELT. ◦ Fix a bug for 2d seatbelt that could occur when a model has both 1d and 2d belts, and a 1d pretensioner of type 2, 3 or 9. ◦ Fix an MPP seatbelt bug that could occur when using a type 9 pretension- er. ◦ Allows shell formulation 9 to be used for 2d seatbelt. It was reset to formu- lation 5 by LS-DYNA, no matter what formulation was input. Now, only formulation 5 and 9 are accepted as input. Other formulations will incur error message. ◦ MPP now supports *ELEMENT_MASS_MATRIX_NODE_(SET). ◦ Added cohesive shell formulation -29. This formulation uses a cohesive midlayer where local direction q1 coincides with the average of the sur- rounding shell normals. This formulation is better suited for simulating normal shear. ◦ Cohesive shell formulation +/-29: Fixed absence of part mass in d3hsp. ◦ Make *TERMINATION_DELETED_SOLIDS work with hex spot weld fail- ures. ◦ Fix incorrect load curve used if large value is used for FC < 0 and/or FCS < 0 in *ELEMENT_SEATBELT_SLIPRING. ◦ Fix incorrect velocity on accelerometer if velocity is prescribed on the rigid body that the accelerometer is at- tached to, and INTOPT = 1 in *ELEMENT_SEATBELT_ACCELEROMETER, and *INITIAL_VELOCITY_GENERATION_START_TIME is used. ◦ Fix incorrect discrete spring behavior when used with adaptivity. INTRODUCTION ◦ Fix input error when using *DEFINE_ELEMENT_DEATH with BOXID > 0 for MPP. ◦ Modify tolerances on error messages SOL+865 and SOL+866 to prevent unnecessary error terminations when translational or rotational mass of a discrete beam was close to zero. ◦ Made the solid element negative volume warning SOL+630 for penta for- mulatgion 15 consistent with the volume calculation in the element. With this change, elements are deleted rather than the job terminating with error SOL+509. ◦ Fixed the default hourglass control for shell form 16. It was defaulting to type 5 hourglass control rather than 8. ◦ Fixed default hourglass control when the *HOURGLASS control card is used but no HG type is specified. We were setting to type 1 instead of 2. Also, fixed the default HG types to match the user's manual for implicit and explicit. ◦ Fixed the fully integrated membrane element (shell ELFORM = 9) when used with NFAIL4 = 1 on *CONTROL_SHELL and there are triangular el- ements in the mesh. Triangular elements were being deleted by the dis- torted element check. ◦ Fixed a divide by zero error that occurred with *SECTION_BEAM, -12, and node 3 was omitted on ELFORM = 6, SCOOR = 12 or *ELEMENT_BEAM, and nodes 1 and 2 are along the global y-direction or z-direction. ◦ Fixed laminated shell theory for type 6 and 7 shell elements when made active by LAMSHT = 3 or 5 on *CONTROL_SHELL. ◦ Added an int.pt. variable for *PART_COMPOSITE_LONG and *PART_COMPOSITE_TSHELL_LONG called SHRFAC which is a scale factor for the out-of-plane shear stress that allows the user to choose the stress distribution through thickness. This was motivated by test data that shows that for large differences is layer shear stiffness, the parabolic as- sumption is poor. ◦ Fixed implicit hourglass stiffness in viscoelastic materials when used with tshell forms 5 or 6. The stiffness was much too small. ◦ Modified tshell type 5 to use the tangent stiffness for calculating the Pois- son's affects and hourglass control for *MAT_024. This makes the behavior softer during buckling which is much more realistic. ◦ Fixed a significant bug in segment based contact when SHLEDG = 1 and SBOPT = 3 or 5 and DEPTH < 45, and shell segments in contact have dif- ferent thicknesses. A penetration check was using incorrect thicknesses causing contact to be detected too late, particularly for edge to surface con- tact. ◦ Improved the time step calculation for triangular tshell elements. The time step was too conservative for elements with significant thickness. This fix does not affect tshell type 7. INTRODUCTION ◦ Fixed all tshells to work with anisotropic thermal strains which can be de- fined by *MAT_ADD_THERMAL. Also, this now works by layer for lay- ered composites. ◦ Enabled tshell form 5 to recalculate shear stiffness scale factors when plas- ticity material models 3, 18, 24, 123, or 165 are included in a composite sec- tion. Prior to this change the scale factors were based on elastic properties so after yielding, the stress distribution was not what was expected. This new capability supports the constant stress option, the parabolic option, and the SHRFAC option on *PART_COMPOSITE_TSHELL_LONG. ◦ Improved tshell 5 when used with mixed materials in the layers. A failure to use the correct Poisson's ratio was causing a less accurate stress tensor. ◦ Modified the time step calculation for tshell forms 3 and 5. A dependence on volumetric strain rate was removed in order to prevent oscillations in the time step which caused stability problems, particularly for tshell 5. (TSHEAR = 1 on *SECTION_TSELL or *PART_COMPOSITE). It was producing a not very constant stress distribution. constant ◦ Fixed option stress tshell shear ◦ Fixed stress and strain output of tshells when the composite material flag CMPFLG is set on *DATABASE_EXTENT_BINARY. The transformation was backwards. mass when *ELEMENT_SHELL_SOURCE_SINK is used. The mass of inactive ele- ments was being included. reported ◦ Fixed d3hsp parts of to ◦ Enabled *MAT_026 and *MAT_126 (HONEYCOMB) to be used with tshell forms 3, 5, and 7. It was initialized incorrectly causing a zero stress. ◦ Added a missing internal energy calculation for tshell form 6. ◦ Enabled tshell forms 1, 2, and 6 to work with material types 54, 55, and 56. ◦ Modified the z-strain distribution in tshell forms 5 and 6 when used in composites with mixed materials that are isotropic. The existing assumed strain scheme was doing a poor job of creating a constant z-stress through the thickness. ◦ Increased the explicit solution time step for thin shell composite elements. The existing method calculated a sound speed using the stiffness from the stiffest layer and dividing it by the average density of all layers. This could be overly conservative for composites with soft layers of low density. The new method uses the average stiffness divided by average density. This is still conservative, but less so. ◦ Corrected rotational inertia of thin shells when layers have mixed density and the outer layers are denser than inner layers. The fix will mostly affect elements that are very thick relative to edge length. ◦ Added support for *ELEMENT_SHELL_SOURCE_SINK to type 2 shells with BWC = 1 on *CONTROL_SHELL. ◦ Prevent (from shell *ELEMENT_SHELL_SOURCE_SINK) from controlling the solution time step. elements inactive INTRODUCTION ◦ Fixed *LOAD_STEADY_STATE_ROLLING when used with shell form 2 (BWC = 1 Belytschko- Wong-Chang warping and *CONTROL_SHELL). The load was not being applied. stiffness ◦ Improved the brick element volume calculation that is used by the option erode elements (ERODE = 1 on *CONTROL_TIMESTEP or PSFAIL.ne.0 on *CONTROL_SOLID). It was not consistent with the element calculation which caused an error termination. ◦ Fixed all tshell forms to work with anisotropic thermal strains which can be defined by *MAT_ADD_THERMAL. Also, this now works by layer for layered composites. ◦ Reworked shell output so that we can correctly output stress in triangular shells when triangle sorting is active, that is when ESORT = 1 or 2 on *CONTROL_SHELL. ◦ *ELEMENT_T/SHELL_COMPOSITE(_LONG) and *PART_COMPOSITE_T/SHELL_(LONG): Permit the definition of zero thickness layers in the stacking sequence. This allows the number of inte- gration points to remain constant even as the number of physical plies var- integration point ies and eases post-processing since a particular corresponds to a physical ply. Such a capability is important when plies are not continuous across a composite structure. To represent a missing ply, set THK to 0.0 for the corresponding integra- tion point and additionally, either set MID = -1 or set PLYID to any non- zero value. Obviously, the PLYID option applies only to the keywords containing LONG. ◦ Implemented sum factorization for 27-node quadratic solid that may in- crease speed by a factor of 2 or 3. ◦ Support second order solid elements (formulations 23,24,25,26) for *SET_NODE_GENERAL. ◦ Invoke consistent mass matrix of 27-node hex element for implicit dynam- ics and eigenvalues. ◦ Reorder node numbering when assembling global stiffness matrix for 27- node hex. This fixes a bug in which it was reported than the implicit 27- node element didn't work ◦ Automatically transfer nodal boundary conditions for newly generated nodes if H8TOH27 option is used in *ELEMENT_SOLID. ◦ Modify initialization of material directions for solid elements. If there are only zeros for all the 6 values in *INITIAL_STRESS_SOLID, then the values from the other input (e.g. *ELEMENT_SOLID_ORTHO) are kept. ◦ Enable *PART_STACKED_ELEMENTS to pile up shell element layers. Be- fore, it was necessary that solid element layers were placed between shell element layers. Now, shell element layers can follow each other directly. Contact definitions have to be done separately. ◦ Allow *PART_STACKED_ELEMENTS to be used in adaptive refinement simulations. INTRODUCTION ◦ Add alternative mass calculation for critical time step estimate of cohesive elements. This hopefully resolves rarely occurring instability issues. Op- tion ICOH on *CONTROL_SOLID is used for that. ◦ Correct the strain calculation for tet formulation 13. This did not affect the stress response, only output of strains. Nodal averaging was not account- ed for. ◦ User defined *SECTION_SHELL/SOLID) *MAT_ADD_EROSION. elements (ELFORM = 101 can now be used to 105 on together with ◦ Add option to define a pull-out in *ELEMENT_BEAM_SOURCE by defining a negative variable FPULL. |FPULL| or refer *DEFINE_CURVE_FUNCTION. *DEFINE_CURVE time curve force vs. can to ◦ Solid tet form 13 supported for all materials in implicit, including a pre- sumable consistency improvement for the future. ◦ The Hughes-Liu beam is supported in *INTEGRATION_BEAM such each integration point may refer to a different part ID and thus have a different coef. Of thermal expansion. See *MAT_ADD_THERMAL_EXPANSION. ◦ Shell types 2 and 16 that combines thermal expansion and thick thermal shells, see *MAT_ADD_THERMAL_EXPANSION and TSHELL on *CONTROL_SHELL, now correctly treat temperature gradient through the thickness to create bending moments. All shell types are to be supported in due time. ◦ *SECTION_BEAM_AISC now provides predefined length conversion fac- tors for specific unit systems. ◦ 3D tet r-adaptivity now supports *DEFINE_BOX_ADAPTIVE. For every adaptive part, users can define multiple boxes where dif- ferent BRMIN & BRMAX (corresponding to RMIN & RMAX in *CONTROL_REMESHING) can be specified for 3D tet remesher to adjust the mesh size. Current implementation does not support LOCAL option. ◦ Fix bug in 3D adaptivity so that users can now have both non-adaptive tshell parts and 3D adaptive parts in one analysis. ◦ Fix the bug in 3D adaptivity so that users can now have both dummy nodes and 3D adaptive parts in one analysis. • *EM (Electromagnetic Solver) ◦ Randles Circuits for Battery Modeling A Randles circuit is an equivalent electrical circuit that consists of an active electrolyte resistance r0 in series with the parallel combination of the capacitance c10 and an impedance r10. The idea of the distrib- INTRODUCTION uted Randles model is to use a certain number of Randles circuits be- tween corresponding nodes on the two current collectors of a battery unit cell. These Randles circuits model the electrochemistry that happens in the electrodes and separator between the current collec- tors. The EM solver can then solve for the EM fields in the current collectors, and the connections between them. Added analysis of distributed Randles circuits to MPP. Added d3plot output for distributed Randles circuits: D3PL_RAND_r0_EM, D3PL_RAND_r10_EM, D3PL_RAND_c10_EM, D3PL_RAND_soc_EM, D3PL_RAND_i_EM, D3PL_RAND_u_EM, D3PL_RAND_v_EM, D3PL_RAND_vc_EM, D3PL_RAND_temperature_EM, D3PL_RAND_P_JHR_EM, D3PL_RAND_P_dudt_EM, D3PL_RAND_i_vector_EM This output can be visualized in LS-PrePost versions 4.3 and 4.5 on the using Post/FriComp/Extend/EM node. separator battery part cell the of Added tshells for EM analysis for use in battery modeling. Added new capability for modeling Randles short, based on *DEFINE_FUNCTION so that the user has a lot of freedom to define where and when the short happens as well as the short resistance. Added a new capability for battery exothermal reactions also based on keyword *RANDLE_EXOTHERMAL_REACTION makes it possible to com- plement the heating of a short circuit created by a short by exother- mal reactions if, for example, the temperature becomes higher than a threshold value. *DEFINE_FUNCTION. new The • FORMING ANALYSIS ◦ Extend *INCLUDE_AUTO_OFFSET to solid and beam elements (draw beads). ◦ Add a for new keyword compensa- tion:*INTERFACE_COMPENSATION_NEW_REFINE_RIGID to refine and break rigid tool mesh along the user supplied trim curves so compensated tool mesh follows exactly the blank mesh (file "disp.tmp"). This needs to be done only once in the beginning of the springback compensation (IT- ER0). springback ◦ *CONTROL_FORMING_ONESTEP: INTRODUCTION Change the default element formulation option for onestep method to QUAD2. Add a new option QUAD to allow quadrilateral elements to be con- sidered. Limit the maximum thickening by using a new variable TSCLMAX for the sheet blank. Set the value of OPTION to a negative value to output the file 'on- estepresult' in large format (E20.0). Calculate and add the damage factor and output to the 6th history variable in the output file "onestepresult". Add the variable for a curve ID to define the fracture strain vs. triaxility. Add another vari- able DMGEXP (damage parameter), as used in GISSMO model. Keep the original coordinates for the onestep output "onestepresults". ◦ Add a new option VECTOR to *CONTROL_FORMING_BESTFIT to output deviation vector (in the format of: NODEID, xdelta, ydelta, zdelta) for each node to its closest target element. The deviation vectors are output under the keyword *NODE_TO_TARGET_VECTOR. ◦ *CONTROL_FORMING_OUTPUT: Output will skip any negative abscissa (Y1) value. When CIDT < 0, the positive value defines the time dependent load curve. ◦ Add a warning compensation *INTERFACE_SPRINGBACK_COMPENSATION to identify which input file (typically the blank with adaptive mesh not output directly by LS- DYNA) has the wrong adaptive constraints. springback in ◦ *INTERFACE_COMPENSATION_3D: turn off the output of nikin file. ◦ *ELEMENT_LANCING: Allow some unused lancing curves to be included in the input. When the gap between the two ends of a lancing curve is not zero, but small enough, then this curve is automatically closed. Allow several parts to be cut during lancing; the parts can be grouped in *SET_PART_LIST, and defined using a negative value IDPT. Specify the distance to bottom dead center as AT and ENDT when the new variable CIVD is defined. Set IREFINE = 1 (default) in lancing, to refine blank mesh automati- cally along the lancing curves. Re-set the adaptive level to be 1 to prevent those elements along the lancing route to be further refined. INTRODUCTION When IREFINE = 1, elements along the lancing curve will be refined to make sure that no adapted nodes exist in the neighborhood. This helps get improved lancing boundary. Change of tolerance for lancing to merge the small elements into big- ger ones. ◦ Add a new keyword to perform trimming after lancing (shell elements on- ly): *DEFINE_LANCE_SEED_POINT_COORDINATES. Maximum of two seed nodes can be defined. ◦ Extend *CONTROL_FORMING_TOLERANC to *MAT_036, *MAT_037, *MAT_125, and *MAT_226. When beta is less than -0.5, there is no necking and no calculation of FI. When beta is greater than 1.0, beta = 1.0/beta. This keyword adds a smoothing method to calculate the strain ratios for a better formability index. ◦ Sandwiched parts (*CONTROL_ADAPTIVE, *DEFINE_CURVE_TRIM): Disable *CONTROL_ADAPTIVE_CURVEs for sandwich parts, since refinement along the curve is automatically done during trimming. Refine the elements along the trimming curve to make sure no slave nodes are be cut by trimming curves. Allow mesh adaptivity. Allow multi-layers of solids. Add a check to the variable IFSAND in *CONTROL_ADAPTIVE for sandwich part to be refined to exclude solid elements. ◦ Solid element trimming (*DEFINE_CURVE_TRIM): Refine those elements along the trimming curve. Improve solid trimmig to allow the trimming of one panel into two panels with two seed nodes. ◦ Add a keyword *CONTROL_FORMING_REMOVE_ADAPTIVE_CONSTRAINTS re- move adaptive constraints on a formed, adapted blank, and replaced them with triangular elements. new to ◦ *DEFINE_CURVE_TRIM_NEW: Allow trimming of tshells. ◦ Add a new keyword:*INTERFACE_WELDLINE_DEVELOPMENT to ob- tain initial weld line from the final part and the final weld line position. When Ioption = -1, convert weld line from its initial position to the fi- nal part. Output the element nodes that intersect the weld line in the final part, and the output file is: affectednd_f.ibo Output the element nodes that intersect the weld line in the initial part, and the output file is: affectednd_i.ibo INTRODUCTION ◦ Add a new variable DT0 to *CONTROL_IMPLICIT_FORMING so there is no need to use *CONTROL_IMPLICIT_GENERAL to specify DT0. ◦ *INTERFACE_BLANKSIZE: Add a new feature DEVELOPMENT option. When ORIENT = 2, then a reference mesh file for the formed part should be included. The calculated and compensated boundary will be based on the ref- erence mesh. Add a new option SCALE_FACTOR that allows the target curve to be moved. This is useful when multiple target curves (e.g. holes) and formed curves are far away from each other. • *FREQUENCY_DOMAIN ◦ Added new keyword *CONTROL_FREQUENCY_DOMAIN to define global control parameters for frequency domain analysis. Currently two parameters are defined: REFGEO: flag for reference geometry in acoustic eigenvalue analysis (either the original geometry at t = 0, or the deformed geometry at the end of transient analysis). MPN: large mass added per node, to be used in large mass method for enforced motion. ◦ *FREQUENCY_DOMAIN_ACOUSTIC_BEM: Enabled wave (*FREQUENCY_DOMAIN_ACOUSTIC_INCIDENT_WAVE) in Ray- leigh method (METHOD = 0). incident using Enabled plot (*FREQUENCY_DOMAIN_ACOUSTIC_FRINGE_PLOT) in Rayleigh method (METHOD = 0). pressure acoustic fringe Fixed bug in running acoustic analysis with multiple boundary con- ditions in MPP. Fixed running MATV (Modal Acoustic Transfer Vector) approach in MPP (*FREQUENCY_DOMAIN_ACOUSTIC_BEM_MATV). Added treatment for triangular elements used in Rayleigh method (METHOD = 0). Added output of acoustic intensity to binary database D3ACS (de- fined by *DATABASE_FREQUENCY_BINARY_D3ACS). Fixed bug in acoustic pressure fringe plot for collocation BEM (METHOD = 3) and dual BEM based on Burton-Miller formulation (METHOD = 4). ◦ *FREQUENCY_DOMAIN_ACOUSTIC_FEM: INTRODUCTION Fixed bug in acoustic analysis by FEM, when dimensions of mass and k (stiffness) matrices are mismatched. ◦ *FREQUENCY_DOMAIN_ACOUSTIC_FRINGE_PLOT: Implemented acoustic fringe plot for MPP for the options PART, PART_SET, and NODE_SET. ◦ *FREQUENCY_DOMAIN_FRF: Added new loading types: VAD1 = 5: enforced velocity by large mass method = 6: enforced acceleration by large mass method = 7: enforced displacement by large mass method = 8: torque = 9: base angular velocity = 10: base angular acceleration = 11: base angular displacement Added rotational dof output for FRF. ◦ *FREQUENCY_DOMAIN_MODE: Added option _EXCLUDE to exclude some eigenmodes in modal su- perposition in frequency domain analysis. ◦ *FREQUENCY_DOMAIN_RANDOM_VIBRATION: Fixed bug in running random vibration with random pressure wave load (VAFLAG = 2) in MPP. Improved random vibration analysis by allowing using complex var- iable cross PSD functions. Previously cross PSD was defined as real variables thus the phase difference was ignored. Added PSD and RMS computation for Von Mises stress in beam ele- ments. ◦ *FREQUENCY_DOMAIN_RESPONSE_SPECTRUM: Added Von Mises stress output for beam elements in database D3SPCM. Corrected computation of response spectrum at an intermediate damping value by interpolating spectra at two adjacent damping values. Now the algorithm is based on ASCE 4-98 standard. ◦ *FREQUENCY_DOMAIN_SSD: Added new loading types: VAD = 5: enforced velocity by large mass method INTRODUCTION = 6: enforced acceleration by large mass method = 7: enforced displacement by large mass method = 8: torque Fix for running SSD fatigue in MPP (affected keyword: *FREQUENCY_DOMAIN_SSD_FATIGUE). Updated ssd computation with local damping, and enabled the re- start feature by reading damping matrix. Implemented ERP (Equivalent Radiated Power, keyword *FREQUENCY_DOMAIN_SSD_ERP) for MPP. ◦ *DATABASE_FREQUENCY_ASCII: Added keyword *DATABASE_FREQUENCY_ASCII_{OPTION} to define the frequency range for writing frequency domain ASCII da- and tabases NODOUT_SSD, ELOUT_PSD. ELOUT_SSD, NODOUT_PSD • *ICFD (Incompressible Fluid Solver) ◦ New ICFD features and major modifications Simple restart is now supported for ICFD. Added damping wave capabilities. See *ICFD_DEFINE_WAVE_DAMPING. Added steady state solver. See *ICFD_CONTROL_GENERAL and *ICFD_CONTROL_STEADY. steady Added state potential flow solver. See *ICFD_CONTROL_GENERAL. Weak thermal coupling for conjugate heat transfer is now possible in See classic monolithic approach. addition to *ICFD_CONTROL_CONJ. the Windkessel boundary conditions are now available for blood flow. See *ICFD_BOUNDARY_WINDKESSEL. It is now possible to output the heat transfer coefficient as a surface variable in LSPP or in ASCII format on segment sets for a subsequent solid-thermal only analysis. See *ICFD_DATABASE_HTC. Two way coupling is now possible with DEM particles. See *ICFD_CONTROL_DEM_COUPLING. Modifications introduced in the SUPG stabilization term used in thermal and conjugate heat transfer problems for improved accuracy and speed. ◦ Additions and modifications to existing ICFD keywords *ICFD_BOUNDARY_FSWAVE: INTRODUCTION Added a boundary condition for wave generation of 2nd order stokes waves with free surfaces *ICFD_CONTROL_FSI: Added a flag which, when turned on will project the nodes of the CFD domain that are at the FSI interface onto the structural mesh. This is recommended for cases with rotation. *ICFD_CONTROL_MESH: Added a flag to allow the user control over whether there will be re- mesh or not. If there is no re-mesh then we can free space used to backup the mesh and lower memory consumption. *ICFD_CONTROL_MESH_MOVE: Added option to force the solver to turn off any mesh displacements. This can be useful in cases where the mesh is static to save a little bit of calculation time. *ICFD_CONTROL_OUTPUT: Added option to support output in Fieldview format, binary and ASCII. When output of the fluid volume mesh is requested, the mesh will be divided into ten distinct parts, grouping elements in ten deciles based on the mesh quality (Part 1 has the best quality elements, part 10 the worst). *ICFD_CONTROL_POROUS: Improvements for RTM problems. *ICFD_CONTROL_TIME: Added an option to define an initial timestep. Added an option to shut off the calculation of Navier Stokes after a certain time leaving only the heat equation. This can be useful to save calculation times in conjugate heat transfer cases where the fluid often reaches steady state before the thermal problem. *ICFD_DATABASE_DRAG: It is now possible to output the force on segment sets in a FSI run di- rectly in LS-DYNA compatible format. This can be useful for a sub- sequent linear FSI analysis running only the solid mechanics part. Added flag to output drag as a surface variable in LSPP. *ICFD_DATABASE_FLUX: Added option to change output frequency *ICFD_DATABASE_NODOUT: The user node IDs are now required rather than the internal node IDs *ICFD_CONTROL_IMPOSED_MOVE: Added the option to choose between imposing the displacements or the velocity. *ICFD_CONTROL_TRANSIENT: Choose implicit time integration scheme for NS. *ICFD_CONTROL_DEM_COUPLING: INTRODUCTION Added a scale factor for the sphere radius in the computation of the DEM force. *ICFD_MODEL_POROUS: Added a scale factor option on the permeability for model 1 and 2. A *DEFINE_FUNCTION can also be used. *MESH_BL: Added option to generate boundary layer mesh using a growth fac- tor. ◦ ICFD bug fixes and minor improvements Fixed bug when multiple *DEFINE_FUNCTIONs were used in an ICFD problem. Only the last one was taken into account. LES turbulence model: fixed van Driest damping issue in the bound- ary layer. LES models can use wall functions. RANS turbulence models: Standard k-epsilon, realizable k-epsilon, Wilcox k-omega uses HRN laws of the wall by default while SST and Spalart Allmaras use LRN. Improvements on the convergence of all those models. The DEM particle volume is now taken into account in free surface problems. Average shear is now output as a surface variable in the d3plots. *ICFD_CONTROL_MONOLITHIC (replaced *ICFD_CONTROL_GENERAL). obsolete is by Added more output for the mesh generation indicating the stage of the meshing process and the amount of elements that are being gen- erated as a multiple of 10000. Added progress % for the extrusion of the mesh during the BL mesh generation. Improvements on the element assemble speed in MPP. Fixed synchronization problem for the last timestep in an FSI prob- lem. More options have been added to the timer output. Correction of the calculation of the flux in *ICFD_DATABASE_FLUX in free surface cases. Boundary layer mesh can go through free-surfaces or mesh size inter- faces. The Center of Gravity of the fluid is output in the icfd_lsvol.dat ASCII file in free surface problems • Implicit (Mechanical) Solver ◦ Enhanced termination of MPP eigensolver when non eigenmodes are found. INTRODUCTION ◦ Implicit was enforcing birth and death times on *BOUNDARY_SPC during dynamic relaxation contrary to the User's Manual. These times are now ignored by implicit during dynamic relaxation. ◦ Corrected output of eigenvalues and frequencies to file eigout for the asymmetric eigenvalue problem. ◦ Enhanced logic that determines when to write out the last state to d3plot for implicit. ◦ Improved error message for reading d3eigv file for *PART_MODES for the case when the user inputs a d3eigv file from a different model than intend- ed. ◦ Corrected the reporting of kinetic and internal energy in file glstat for im- plicit. ◦ Applied corrections to tied contact in implicit (MPP). This affects slave nodes coming from other processes. ◦ Corrected output to file d3iter (implicit nonlinear search vectors) for re- start. ◦ Enhanced termination process when the implicit solver determined an ear- ly termination. ◦ When implicit springback was following an explicit transient step, the im- plicit keywords with the _SPR were not properly handled. This is now corrected. ◦ Added a warning of *CONSTRAINED_RIGID_BODY_STOPPERS and the Lagrange multiplier formulation for joints (*CONTROL_RIGID) for explicit. The warning rec- ommends switching to the penalty joint formulation. combined about use the ◦ Applied numerous bug fixes to the implicit solver associated with *CONSTRAINED_INTERPOLATION where there are lots of independent degrees-of-freedom. ◦ Corrected initialization of MPP tied contact with implicit mechanics when the implicit phase follows explicit dynamic relaxation. ◦ Fixed an implicit problem where a linear implicit analysis follows inertia relief computation. ◦ Added gathering of damping terms from discrete elements from implicit especially for FRF computations and matrix dumping. ◦ Fixed Implicit for the case of multi-step Linear (NSOLVR = 1) with Inter- mittent Eigenvalue Computation. ◦ Corrected the output to d3iter when 10-noded tets are present. ◦ Keypoints specified in *CONTROL_IMPLICIT_AUTO are now enforced at the initial time step and on restart from explicit. ◦ Skip frequency damping during implicit static dynamic relaxation, i.e. IDRFLAG > 5. ◦ *CONTROL_IMPLICIT_ROTATIONAL_DYNAMICS: The VID of the rotating axis can now be defined by both *DEFINE_VECTOR and *DEFINE_VECTOR_NODES. It enables the INTRODUCTION movement of the rotating axis. Previously, only *DEFINE_VECTOR could be used to define the VID. The rotational dynamics now work in MPP. ◦ Shell forms 23 and 24 (high order shells), 1D seatbelts, Hughes-Liu and spotweld beams (types 1 and 9) are now supported with the implicit accu- racy option (IACC = 1 in *CONTROL_ACCURACY) to render strong ob- jectivity for large rigid body rotations. Also, shell type 16 is supported with implicit accuracy option, resulting in forms 16 and -16 giving the same solution. ◦ Translational and generalized stiffness joints are now strongly objective for implicit analysis. See CONSTRAINED_JOINT_STIFFNESS.... ◦ In implicit it may happen that the initial loads are zero, for instance in forming problems. In addition, the goal is to move a tool in contact with a workpiece, and the way line search and convergence works, it is hard to get things going. We now attempt to handle this situation by automatical- ly associating an augmented load to the prescribed motion simply to get off the ground. ◦ New tolerances on maximum norms are introduced for convergence in implicit: ratio of max displacement/energy/residual, and absolute values of nodal and rigid body translation/rotational residual can be specified. See DNORM.LT.0 on *CONTROL_IMPLICIT_SOLUTION for defining an additional card for these parameters DMTOL, EMTOL and RMTOL. Fur- thermore, maximum absolute tolerances on individual nodal or rigid body parameters can be set on NTTOL, NRTOL, RTTOL and RRTOL on the same card. ◦ If ALPHA < 0 on first *CONTROL_IMPLICIT_DYNAMICS card, the HHT implicit time integration scheme is activated. • *INITIAL ◦ Fix *INITIAL_VELOCITY_GENERATION with *INCLUDE_TRANSFORM, which was broken due to misplaced condi- tionals in r100504. when used ◦ Fix 3 bugs for *INITIAL_VELOCITY_GENERATION involving omega > 0 and icid > 0: When nx = -999. Now the directional cosine defined by node NY to node NZ will be the final direction to rotate about. In other words, the direction from node NY to node NZ will not be projected along icid any more. When nx != -999, (xc,yc,zc) should not be rotated along icid, since (xc,yc,zc) are global coordinates. When is *INCLUDE_TRANSFORM, (xc,yc,zc) is transformed. *INITIAL_VELOCITY_GENERATION 1-182 (INTRODUCTION) INTRODUCTION ◦ Add of the time option ramping for *INITIAL_FOAM_REFERENCE_GEOMETRY. The solid elements with reference geometry and ndtrrg > 0 will restore its reference geometry in ndtrrg time steps. incorrect in velocity *INITIAL_VELOCITY_GENERATION, and rotational velocity, omega, is not zero and *PART_INERTIA is also present. ICID.ne.0 ndtrrg, initial steps, when ◦ Fix ◦ Add variable IZSHEAR in *INITIAL_STRESS_SECTION to initialize shear stress. ◦ Fix incorrect initial velocity for *INITIAL_VELOCITY if IRIGID = -2 and ICID > 0. ◦ Fix incorrect NPLANE and NTHICK for *INITIAL_STRESS_SHELL when writing dynain for shell type 9. ◦ Fix *INITIAL_STRAIN_SHELL output to dynain for shell types 12 to 15 in 2D analysis. Write out strain at only 1 intg point if INTSTRN = 0 in *INTERFACE_SPRINGBACK_LSDYNA and all strains at all 4 intg points if INTSTRN = 1 and nip = 4 in *SECTION_SHELL. the ◦ Skip transformation of ICID > 0 and *INCLUDE_TRANSFORM is used to transform the keyword input file with the *INITIAL_VELOCITY.... keyword. Also echo warning message, KEY+1109, that the transformation will be skipped since icid is specified. ◦ Fix incorrect transformation of *DEFINE_BOX which results in incorrect initial velocities if initial velocities if the box is used in *INITIAL_VELOCITY. ◦ Fixed *INITIAL_STRESS_DEPTH when used with 2D plane strain and ax- isymmetric elements. The prestress was being zeroed. ◦ Improved the precision of the initial deformation calculation for *INITIAL_FOAM_REFERENCE_GEOMETRY in the single precision ver- sion. ◦ Fixed stress initialization (*INITIAL_STRESS_SECTION) for type 13 tet el- ements. The pressure smoothing was causing incorrect pressure values in the elements adjacent to the prescribed elements. ◦ Add _SET option to *INITIAL_STRESS_SOLID for element sets. ◦ Fix bug in 3D adaptivity *INITIAL_TEMPERATURE for adaptive parts. that users so can now define • Isogeometric Elements ◦ The stability of the trimmed NURBS shell patches has been improved. ◦ Add *LOAD_NURBS_SHELL to apply traction type loading directly on the surface of NURBS shell. ◦ Users can use the PART option of *SET_SEGMENT_GENERAL to define segment set of a NURBS patch. The segment set will contain all segments of interpolated null shell elements. ◦ *ELEMENT_SOLID_NURBS_PATCH: INTRODUCTION Isogeometric solid analysis implemented for MPP. Isogeometric solid analysis implemented for SMP with multiple CPUs, including consistency (ncpu < 0). Activate user-defined materials for isogeometric solid. ◦ *ELEMENT_SHELL_NURBS_PATCH: Isogeometric shell analysis now implemented for SMP with multiple CPUs, including consistency (ncpu < 0). Add a power iteration method to get the maximum eigen-frequency for each isogeometric element. This will be used to set a reasonable time step for trimmed elements. ◦ *ELEMENT_SHELL_NURBS_PATCH: Changed the way of projecting the results from isogeometric (NURBS) elements to the interpolation elements. Now a background mesh, spanned over the locations of the integration points of the iso- geometric (NURBS) elements serves as basis to interpolate results from the integration points to the centroid of the interpolation ele- ments. This change may lead to slightly different post-processing re- sults in the interpolation elements. ◦ Add support for trimmed NURBS to work in single precision. Anyway, it is still recommended to use double precision versions for trimmed NURBS patches. ◦ Add post-processing of strains and thickness for interpolation shells. • *LOAD ◦ Fixed bugs affecting discrete beam elements (ELFORM = 6) when used with staged construction. Here, "dormant" refers to elements that have not on as yet *DEFINE_STAGED_CONSTRUCTION_PART. defined become active Dormant discrete beams could still control the timestep and attract mass-scaling, when they should not do so. Dormant discrete beams reaching a failure criterion defined on the *MAT card were deleted, when they should not be. The displacements output included displacements occurring while the elements were dormant. Now, the output displacements are reset to zero at the moment the element be- comes active. INTRODUCTION ◦ Fixed bug on *CONTROL_STAGED_CONSTRUCTION had been left blank, and Dy- namic Relaxation was active, an error termination occurred. Construction: Staged FACT in if ◦ Fixed bug: *LOAD_GRAVITY_PART (and also gravity loading applied by *DEFINE_STAGED_CONSTRUCTION_PART) was failing to account for non-structural mass when load: NSM on *SECTION_BEAM and MAREA on *SECTION_SHELL. calculating gravity ◦ Fixed bug in *LOAD_VOLUME_LOSS: inconsistent results when run in SMP parallel. ◦ Fix bugs affecting *LOAD_SEGMENT_FILE: Remove LOAD_SEGMENT_FILE file size limit (It used to be 200M). Apply correct pressure on the shared boundary between processors. ◦ Fix GRAV = 1 in *PART which was not were not working correctly with *LOAD_DENSITY_DEPTH. Make *LOAD_DENSITY_DEPTH work for Lagrangian 2D elements. ◦ Fix insufficient memory error,SOL+659, when using *LOAD_ERODING_PART_SET with MPP. ◦ Fix incorrect loading when using *LOAD_ERODING_PART_SET with BOXID defined. ◦ Added *LOAD_SUPERPLASTIC_FORMING for implicit analysis. ◦ *LOAD_SUPERPLASTIC_FORMING box option now works in MPP. • *MAT and *EOS ◦ *MAT_197 (*MAT_SEISMIC_ISOLATOR) could become unstable when the parameter DAMP was left at its default value. A workaround was to input DAMP as a small value such as 0.05. The timestep for *MAT_197 is now smaller than previously, irrespective of the DAMP setting, and the behav- ior is now stable even if DAMP is left at the default. ◦ Fixed bug: Timestep calculation was wrong for *MAT_089 solid elements. Response could be unstable especially for higher values of Poisson's ratio, e.g. 0.4. ◦ Fixed bug: An error trap was wrongly preventing ELFORM = 15 for elements with (*MAT_ARUP_ADHESIVE). Wedge *MAT_169 ELFORM = 15 are now permitted. ◦ *MAT_172 (*MAT_CONCRETE_EC2): Note that items (1) and (2) below can lead to different results compared to previous versions of LS-DYNA. (1) The number of potential cracks in MAT_172 shell elements has been increased from 2 to 4. MAT_172 uses a fixed crack model: once the first crack forms, it remains at the same fixed angle relative to the element axes. Further cracks can then form only at pre-defined an- INTRODUCTION gles to the first crack. Previously, only one further crack could form, at 90 degrees to the first crack. Thus, if the loading direction subse- quently changed so that the principal tension is at 45 degrees to the first crack, that stress could exceed the user-defined tensile strength by a considerable margin. Now, further cracks may form at 90, +45 and -45 degrees to the first crack. Although the maximum principal stress can still exceed the user-defined tensile strength, the "error" is much reduced. There is an option to revert to the 2-crack model as in R9 (to do this, add 100 to TYPEC). (2) Add element erosion to MAT_172. This change may lead to dif- ferent results compared to previous versions, because erosion strain limits are now added by default. Elements are now deleted when crack-opening strain becomes very large, or the material is crushed beyond the spalling limit. Plastic strain in the rebar is considered too. Previously, these elements that have passed the point of being able to generate any stress to resist further deformation would remain in the calculation, and sometimes showed very large non-physical defor- mations and could even cause error terminations. Such elements would now be deleted automatically. Default values are present for the erosion strains but these can be overridden in the input data, see new input fields ERODET, ERODEC, ERODER. (3) New history variables 10,11,12 (maximum value so far of through- thickness shear stress). This is useful for checking results because MAT_172 cracks only in response to in-plane stress; before cracking occurs, the through-thickness shear capacity is unlimited. The data components are: Ex History Variable 10 - maximum out of 11 and 12 Ex History Variable 11 - maximum absolute value of YZ shear stress Ex History Variable 12 - maximum absolute value of ZX shear stress These are in the element local axis system. Note that these variables are written only if TYPESC is zero or omitted. TYPESC is a pre- existing capability that requests a different type of shear check. (4) Fixed bug. Elastic stiffness for MAT_172 beams was not as de- scribed in the manual, and the axial response could sometimes be- come unstable. The bug did not affect shell elements, only beams. (5) *MAT_172 can now handle models with temperatures defined in Kelvin (necessary if the model also has heat transfer by radiation). *MAT_172 has thermally-sensitive material properties hard-wired to assume temperatures in Centigrade. A new input TMPOFF in *MAT_172 offsets the model temperatures before calculating the ma- terial properties. (6) When the input parameter AGGSZ is defined, the maximum shear stress that can be transferred across closed cracks is calculated from a formula that has tensile strength and compressive stress as inputs. In MAT_172, the tensile strength of concrete is reduced when compres- INTRODUCTION sive damage has occurred . Up to now, compressive damage was therefore influencing the maximum shear across cracks. However, the Norwegian standard from which the shear formula is taken treats the tensile strength as a constant. There- fore, for the purpose of calculating the maximum shear stress across closed cracks only, the compressive damage effect is now ignored. (7) Added capability for water pressure in cracks, for offshore appli- cations. The water pressure is calculated from the depth of the ele- ment below the water surface (calculated from the z-coordinate). The water pressure is applied as a compressive stress perpendicular to the plane of any crack in the element. See new input fields WRO_G and ZSURF. ◦ *MAT_119 (*MAT__GENERAL_NONLINEAR_6DOF_DISCRETE_BEAM): Fixed bug in UNLOAD option 2. The bug occurs if an unloading curve has been left zero (e.g. LCIDTUR) while the corresponding loading curve was non-zero (e.g. LCIDTR), and UNLOAD = 2. Depending on the computer system, the symptoms could be harmless or the code could crash. Now, if the unloading curve is left blank, it is assumed to be the same as the load- ing curve i.e. load and unload up and down the same curve. That behav- ior was already implemented for UNLOAD = 1. ◦ Added Equation Of State 19 (*EOS_MURNAGHAN). Used extensively for fluid modeling in SPH through Weakly-Compressible formulation, in con- junction with SPH formulations 15 (fluid form) and 16 (normalized fluid form). ◦ *MAT_ADD_FATIGUE: Added a new form of Basquin equation to define material's SN curve: LCID = -3: S = a*N^b, where a and b are material con- stants. ◦ Add the option of A0REF for *MAT_FABRIC. That allows the option of using reference geometry to calculate A0 for the purpose of porosity leak- age calculation. ◦ Add optional parameter DVMIN for *MAT_ADD_PORE_AIR to define the min volume ratio change to trigger pore air flow analysis. ◦ *DEFINE_HAZ_PROPERTIES: ◦ Distance of shell from the weld center is treated consistently under MPP and the shell material's yield stress is scaled properly. ◦ *MAT_168 and *MAT_279: Fixed support for element erosion. ◦ *MAT_092: Improved of implicit convergence for shells. ◦ *MAT_224: Fixed bug where wrong shear modulus was used in EOS. ◦ *MAT_270: Increased stability for thickness strain iterations for shells. ◦ *MAT_240: Added support for cohesive shell formulation +/-29. ◦ Scale load curve, LCSRS, of *MAT_ADD_EROSION when used with *INCLUDE_TRANSFORM. INTRODUCTION ◦ Fix incorrect using results *MAT_TABULATED_JOHNSON_COOK/*MAT_224 with table LCKT de- fined and the first abscissa value, temperature, is negative. table ◦ Fix spurious element deletion when using for LCF when *MAT_TABULATED_JOHNSON_COOK/*MAT_224 *MAT_TABULATED_JOHNSON_COOK_GYS/*MAT_224GYS. in and ◦ Error terminate with message, KEY+1142, if *MAT_ADD_EROSION is ap- plied to resultant materials 28,116,117,118,130,139,166,170 and 98(with 1 intg point). ◦ Increase robustness of *MAT_033/*MAT_BARLAT_ANISOTROPIC_PLASTICITY for solids. ◦ Fix input error when *MAT_ELASTIC_WITH_VISCOSITY_CURVE/*MAT_060c LCID = 0. using when ◦ Fix seg fault when using shell type 15, axisymmetric volume weighted, with *MAT_ADD_EROSION and also materials with equation-of-states. ◦ Store computed yield strength as history variable #6 for *MAT_255. ◦ Fix for inconsistency *MAT_MODIFIED_PIECEWISE_LINEAR_PLASTICITY/*MAT_123 when ncpu < 0. ◦ Include original volume output to dynain file for 2D analysis when materi- als with an equation-of-state are used. This is needed to compute the de- formation gradient when initializing a run using the dynain file. ◦ Fix improper stress initialization using *INITIAL_STRESS_SHELL via dynain for *MAT_018/*MAT_POWER_LAW_PLASTICITY with VP = 1.0. ◦ Make for *MAT_170/*MAT_RESULTANT_ANISOTROPIC, i.e. with material coor- dinate system using *DEFINE_COORDINATE_(OPTION). AOPT < 0 work ◦ Fix incorrect operation *MAT_MODIFIED_PIECEWISE_LINEAR_PLASTICITY/*MAT_124 *MAT_PLASTICITY_WITH_DAMAGE/*MAT_081/*MAT_082. TDEL of for and ◦ Fix incorrect damping when using *DAMPING_PART_STIFFNESS for and *MAT_16/*MAT_PSEUDO_TENSOR *EOS_TABULATED_COMPACTION. ◦ Fix incorrect computation of bulk modulus which caused complex sound speed error when using *EOS_TABULATED/EOS_09 with tabulated in- put. ◦ Fix moving part with *MAT_220 during dynamic relaxation when veloci- ties are initialized. ◦ Fix for *MAT_065/*MAT_MODIFIED_ZERILLI_ARMSTRONG for shells when VP = 1. convergence issue ◦ Error terminate with message, KEY+1115, if _STOCHASTIC option is in- no for materials 10,15,24,81,98, voked 123 but or INTRODUCTION *DEFINE_STOCHASTIC_VARIATION or *DEFINE_HAZ_PROPERTIES keyword is present in the input file. ◦ Fix spurious error termination when using *DEFINE_HAZ_PROPERTIES with adpativity. ◦ Fix incorrect results or seg fault for *MAT_FU_CHANG_FOAM/*MAT_083 if KCON > 0.0 and TBID.ne.0. ◦ If SIGY = 0 and S = 0 in *MAT_DAMAGE_2/*MAT_105, set S = EPS1/200, where EPS1 is the first point of yield stress input or the first ordinate point of the LCSS curve. ◦ Allow *MAT_ENHANCED_COMPOSITE_DAMAGE/*MAT_054 failure mechanism to work together with *MAT_ADD_EROSION for shells. ◦ Fix incorrect erosion behavior if *MAT_ADD_EROSION is used with fail- for ure *MAT_123/*MAT_MODIFIED_PIECEWISE_LINEAR_PLASTICITY. defined criteria ◦ Implement *MAT_FHWA_SOIL/*MAT_147 for 2D analysis, shell types 13, 14 and 15. ◦ Implement scaling of failure strain for *MAT_MODIFIED_PIECEWISE_LINEAR_PLASTICITY_STOCHASTIC/* MAT_123_STOCHASTIC for shells. ◦ Fix for *MAT_LINEAR_ELASTIC_DISCRETE_BEAM/*MAT_066 when using damping with implicit (static) to explicit switching. behavior incorrect ◦ Fixed *MAT_FABRIC/*MAT_034 with the negative unloading curve op- tion. When searching for the intersection point of the load and unload curves, and extrapolation of one of the curves was needed to find the inter- section point, the extrapolated stress was calculated incorrectly causing unpredictable behavior. ◦ Fixed fabric material forms 0 and 1 when used with a reference geometry. There were two problems, both occurring when there are mixed quad and triangular elements in the same block. A flaw in the strain calculation was leading to possible NaN forces in the elements. When a reference geome- try was not used, the forces from triangular elements in mixed element blocks were 2 times too high. ◦ Added a new option for *MAT_SPOTWELD called FMODE. The FMODE option is available for DMGOPT = 10, 11, and 12. When the failure func- tion is reached, and when FMODE > 0.0 and < 1.0, the value of FMODE will determine if a weld will fail immediately, or will have damage initiat- ed. The failure function may include axial, shear, bending and torsion terms. If the sum of the squares of the shear and torsion terms divided by the sum of the square of all terms is greater than FMODE, then the weld will fail immediately. Otherwise, damage will be initiated. ◦ Enabled OPT = -1 on *MAT_SPOTWELD for brick elements which had not worked previously. Also, fixed TRUE_T when used with brick element forms 0, 1, and -1. INTRODUCTION ◦ Fixed spotwelds with DMGOPT = 12 by removing warning STR+1327 which made it impossible to set a small value of RS without triggering this warning, or without setting EFAIL smaller. Setting EFAIL small however could lead to damage initiation by plastic strain when the user wanted on- ly initiation by the failure function. ◦ If DMGOPT = 10, 11, or 12 and EFAIL = 0, on *MAT_SPOTWELD, damage will now initiate only by the failure function. If EFAIL > 0, then damage will initiate be either then failure function or when plastic strain exceeds EFAIL. Prior to this version, damage could initiate when plastic strain ex- ceeds zero if the user set EFAIL = 0. This behavior is still true for DMGOPT = 0, 1, or 2, but no longer for DMGOPT = 10, 11, or 12. ◦ Allow solid spot welds and solid spot weld assemblies to have up to 300 points in the running average that is used to smooth the failure function. In other words, up to NF = 300 is possible. ◦ Fixed a problem with brick spot weld assemblies when OPT = 0 failure is used without defining any weld resultant values. Welds were being im- mediately deleted. ◦ Added new PID option for *DEFINE_SPOTWELD_FAILURE (applies to *MAT_SPOTWELD, OPT = 10). Changes the Card 3 input for static strength values to use part set ID’s rather than material ID’s. ◦ Modified shell *MAT_214/*MAT_DRY_FABRIC to calculate fiber strains based on the current distance between the points where the fibers intersect with the element edges. Previously, they were calculated from the rate-of- deformation, but this was not as accurate as the new total strain measure. ◦ Fixed unit scaling for GAMAB1 and GAMAB2 on *MAT_DRY_FABRIC. ◦ Reworked We were incorrectly transforming them as stress. stress in *MAT_225/*MAT_VISCOPLASITC_MIXED_HARDENING to prevent a divide by zero. update plastic the ◦ Enabled *MAT_ADD_EROSION to be used with beams that have user de- fined integration. Memory allocation was fixed to prevent memory errors. ◦ Fixed *MAT_106 when used with tshell form 5 or 6. The elastic constants used in the assumed strain field were not reasonable. ◦ Fix issue that could have led to problems using *MAT_054 (or *MAT_058 or *MAT_158) in combination with TFAIL/TSIZE.gt.0.0 and damping. ◦ *MAT_054 - *MAT_ENHANCED_COMPOSITE_DAMAGE: Add possibility to use failure criterion in *MAT_054 for solids in a transversal isotropic manner. It is assumed that the material 1- direction is the main axis and that the behavior in the 2-3 plane is iso- tropic. This feature is invoked by setting TI = 1 in *MAT_054. ◦ *MAT_058 - *MAT_LAMINATED_COMPOSITE_FABRIC: INTRODUCTION Bugfix for shear stiffness behavior in *MAT_058 when using a table definition for GAB and only providing stress-strain-curves for posi- tive shear. Bugfix for strain-rate dependent stiffness behavior in *MAT_058 when using a table definition for EA, EB or GAB under compressive loading. Add default values for strengths (XT,XC,YT,YC,SC) 1.e+16 for *MAT_058. If no values for the strengths were defined, unpredictable things could have happened. ◦ *MAT_138 - *MAT_COHESIVE_MIXED_MODE: Store total mixed-mode and normal separation (delta_II & delta_I) on history variables 1&2 *MAT_COHESIVE_MIXED_MODE (*MAT_138). This is only for post-processing and should not lead to any changes in the results. for ◦ *MAT_157 - *MAT_ANISOTROPIC_ELASTIC_PLASTIC: Add Tsai-Hill failure criterion (EXTRA = 2). Allow strain-rate values dependent (XT,XC,YT,YC,ZT,ZC,SXY,SYZ,SZX) using *DEFINE_CURVE. This is available for Tsai-Wu (EXTRA = 1) and Tsai-Hill. strength Fixed bug in using *MAT_157 with IHIS.gt.0 for shells. Thickness strain update d3 was not correct and plasticity algorithm may have failed. Add additional option to IHIS in *MAT_157 for SHELLs. Now also the strength values (XT,XC,YT,YC,SXY) may be initialized via *INITIAL_STRESS_SHELL. See variable IHIS and remarks in the User's Manual for details of initializing various blocks of material pa- rameters. ◦ *MAT_215 - *MAT_4A_MICROMEC: Add new material *MAT_215 that is a micromechanical material model that distinguishes between a fiber/inclusion and a matrix ma- terial. The material is intended for anisotropic composite materials, especially for short (SFRT) and long fiber thermoplastics (LFRT). This model is available for shells, tshells and solids. ◦ *MAT_225 - *MAT_VISCOPLASTIC_MIXED_HARDENING: Fixed *MAT_225 (*MAT_VISCOPLASTIC_MIXED_HARDENING) when using a table for LCSS together with kinematic hardening. bug in INTRODUCTION ◦ *MAT_261 - *MAT_LAMINATED_FRACTURE_DAIMLER_PINHO: *MAT_262 - *MAT_LAMINATED_FRACTURE_DAIMLER_CAMANHO: Allow for table input for mats 261/262.Table represents fracture toughness vs. element length vs. strain rate (shells, tshells, solids) mats toughness values 261/262 fracture when bug in Fixed together with RYLEN = 2 using in *DAMPING_PART_STIFFNESS *CONTROL_ENERGY. Correct shear failure behavior in *MAT_262. This will most probably have no effect to any real application, but could be seen in very spe- cial 1-element tests. ◦ Changed storage *MAT_249 (*MAT_REINFORCED_THERMOPLASTIC). A new variable POSTV con- trols which variables are written and at what history variable location in d3plot. variables history for of ◦ *MAT_254 (*MAT_GENERALIZED_PHASE_CHANGE) can now be used with shell elements and thermal thick shells. ◦ Added flag 'EZDEF' to *MAT_249_UDFIBER. In this case the last row of the deformation gradient is replaced by 0-0-1. damage limitation opt. ◦ Add curve/table LCDLIM for *MAT_ADD_GENERALIZED_DAMAGE. ◦ Add pre-defined damage tensors option PDDT to *MAT_ADD_GENERALIZED_DAMAGE. ◦ *MAT_ADD_GENERALIZED_DAMAGE now works for solid elements (only shells in R9). ◦ Add optional failure criterion FFCAP to *MAT_100 with OPT = -1 or 0. ◦ Enable *MAT_ADD_COHESIVE to be used in implicit analysis. ◦ Add alternative version of *MAT_280 invoked by new flag on 1st card. It is a physically based damage model with 4 new parameters. ◦ Enable *DEFINE_CONNECTION_PROPERTIES' option PROPRUL>=2 to be used with spotweld clusters, i.e. not only 1 hex element but several (via *DEFINE_HEX_SPOTWELD_ASSEMBLY on *CONTROL_SPOTWELD_BEAM). RPBHX > 1 or ◦ Enable *MAT_ADD_EROSION to be safely used with material models that have more than 119 history variables, for now the new limit is 169 (e.g. necessary for *MAT_157 with IHIS = 7). ◦ Add Tsai-Wu failure criterion to *MAT_157 for solid and shell elements invoked by EXTRA = 1 on card 6 and corresponding parameters on cards 8 and 9. ◦ Add viscoelastic option to *MAT_187 (SAMP-1). Rate dependent Young's modulus and associated settings can be defined on new optional card 5. ◦ Add new option IRNG for *DEFINE_STOCHASTIC_VARIATION to gov- ern random number generation (deterministic or true random). INTRODUCTION ◦ Add option to define element size dependent parameters EN and SN for *MAT_120 and *MAT_120_JC by setting them to negative values (curves). ◦ Minor improvements for *MAT_252: Optional output of damage initiation information and more post-processing history variables. ◦ If the first abscissa value of *MAT_224's failure strain curve LCG is nega- tive, it is assumed that all abscissa values are natural logarithms of a strain rate. ◦ Put *MAT_100_DA's "failure function" value to history variable 18. ◦ Add optional in-plane failure strain to *MAT_169 (ARUP_ADHESIVE): new input parameter FSIP. ◦ *MAT_USER_DEFINED_MATERIAL_MODELS now provides a few more variables for cohesive elements, i.e. additional arguments in subroutines umatXXc: temperature, element size, implicit rejection flag, integration point identifier, and total number of integration points. ◦ A modified version of the 3-parameter Barlat model (*MAT_036) is intro- duced as *MAT_EXTENDED_3-PARAMETER_BARLAT. In this model, hardening in 00, 45, 90, biaxial and shear can be specified as load curves. Furthermore, r-values in 00, 45, 90, biaxial and shear can be specified in terms of load curves vs plastic strain or constants. This is an extension of hardening law 7 of the original 3-parameter Barlat model. version implicit ◦ Improve of *MAT_098/*MAT_SIMPLIFIED_JOHNSON_COOK. ◦ *MAT_181/*MAT_SIMPLIFIED_RUBBER/FOAM is now supported for 2D implicit simulations. ◦ Fixed issue in which *MAT_WINFRITH_CONCRETE wrote d3crack data too frequently. ◦ *EOS_JWL now has an AFTERBURN option. This adds afterburn energy to the EOS, where the energy can be added at a constant or linear rate, or can be added according to Miller's extension. ◦ ◦ *MAT_084 (*MAT_WINFRITH_CONCRETE) with predefined units (CONM < 0) is now transformed correctly with *INCLUDE_TRANSFORM. ◦ User-defined materials for Hughes-Liu beams can now be used with im- plicit analysis by defining the appropriate tangent modulus in the supplied routine urtanb. ◦ User-defined cohesive materials can now be used with implicit analysis by defining the appropriate tangent stiffness. ◦ *MODULE for user-defined materials and other user-defined capabilities: A new command line option "module = filename" is added to load one module file without changing the input deck. It provides back compatibility to input deck without the MODULE keywords. The system paths defined in LD_LIBRARY_PATH are also included for searching module files for those filenames start with "+". INTRODUCTION ◦ Add shell implementation to *MAT_277 (*MAT_ADHESIVE_CURING_VISCOELASTIC). ◦ Add *MAT_278 for carbon fiber prepreg compression forming simulation. This material model is available for both solid and shell formulations. ◦ Add *MAT_293 non-orthogonal material model for carbon fiber prepreg forming simulation. This material model is only available for shell formu- lations. ◦ *MAT_260A: Extend *MAT_260A to include solid elements. Add a new option XUE for Xue's fracture criteria/theory for *MAT_M260A (solid elements only). ◦ *MAT_260B: Set default values for P's and G's in *MAT_260B. Add a length scale to the fracture limit. The fracture limit strongly depends on the length scale in the measurement. Add a new fracture criterion to *MAT_260B (Xue and Wierzbicki, Int. J. solids and Structures 46 (2009) 1423-1435). When the option XUE is activated, an additional card is needed, for example: $ ef0 plim q gama m 0.70 925.7 0.970 0.296 2.04 ◦ *MAT_037: Improve *MAT_037 with negative R value in implicit calculation. The modification will allow the implicit method stress calculation to be more accurate. Add a new option NLP2 to calculate formability index in *MAT_037. The previous method (option NLP_FAILURE) was based on the ef- fective strain method, which assumes that necking happens at one in- stant. In fact, it might happen over a longer process. The new method calculates the damage accumulation. ◦ Add *MAT_165B (*MAT_PLASTIC_NONLINEAR_KINEMATIC_B) for shells and solids. • MPP ◦ Fix the report of decomp balance (shown as "Normalized element costs as- signed during decomposition" in the d3hsp file), which was broken in r109760 ◦ MPP decomposition has not been properly balanced since r112652 due to a bug in that revision INTRODUCTION ◦ Fix MPP SYNC error due to inconsistent summation in *CONTACT_SLIDING_ONLY_PENALTY. ◦ Allow real values as the scale multipliers for "memory=" on the command line. For example, "memory = 2.5G memory2 = 1.1G" and the like. ◦ MPP: fix support for nlq setting in *CONTROL_SOLUTION which was not being honored on processors other than 0. ◦ Significant improvements in MPP groupable routines for FORMING con- tact. ◦ MPP: increase contact release distance for SINGLE_SURFACE contacts in the case of a node coming into contact with a solid element. The previous interpretation was releasing when the contact penetration was 0.5*solid thickness, but now when the node passes below the solid surface by 0.5*solid thickness (which is different by the half thickness of the slave ma- terial, in the case of a shell slave node). ◦ MPP: fix for viscous damping in automatic tiebreak contact. ◦ Implement new bucket sort based extent testing for MPP single surface contact. ◦ Added MPP support for *CONTACT_AUTOMATIC_SURFACE_TO_SURFACE_LUBRICATION. ◦ Fixed *CONTROL_MPP_PFILE so that it honors ID offsets from *INCLUDE_TRANSFORM for parts, part sets, and contact IDs referenced in "decomp { region {" specifications. ◦ Furthermore, such a region can contain a "local" designation, in which case the decomposition of that region will be done in the coordinate system lo- cal to the include file, not the global system. For example: ◦ *CONTROL_MPP_PFILE decomp { region { partset 12 local c2r 30 0 -30 0 1 0 1 0 0 } } would apply the c2r transformation in the coordinate system of the include file, which wasn't previously possible. The local option can be useful even if there are no such transformations, as the "cubes" that the de- composition uses will be oriented in the coordinate system of the include file, not the global system. ◦ Furthermore, the following decomposition related keywords now have a _LOCAL option, which has the same effect: *CONTROL_MPP_DECOMPOSITION_PARTS_DISTRIBUTE_LOCA L *CONTROL_MPP_DECOMPOSITION_PARTSET_DISTRIBUTE_LO CAL *CONTROL_MPP_DECOMPOSITION_ARRANGE_PARTS_LOCAL *CONTROL_MPP_DECOMPOSITION_CONTACT_DISTRIBUTE_L OCAL ◦ MPP job performance profiles are output to both .csv and .xy files. • OUTPUT INTRODUCTION ◦ Fix for writing d3plot file when individual output states exceed 8GB in single precision ◦ Added new option *INTERFACE_SPRINGBACK_EXCLUDE to exclude selected portions from the generated dynain file. ◦ Add a new option to *INTERFACE_COMPONENT_FILE to output only 3 degrees of freedom to the file even if the current model has 6. ◦ Fix missing plastic strain *DATABASE_EXTENT_BINARY *INTERFACE_SPRINGBACK. tensors is in d3plot when STRFLG set INTSTRN = 1 and in in ◦ Fix no output to bndout when run with q = remap even though the key- word *DATABASE_BNDOUT was present in the remap run but was not present in the initial run. ◦ Fix d3plot output frequency which was different from the dt specified in is *DATABASE_BINARY_D3PLOT when *CONTACT_AUTO_MOVE used. ◦ Fix stress output to elout for solid elements which was in the global coor- in in coordinates when CMPFLG = 1 dinates *DATABASE_EXTENT_BINARY *DATABASE_ELOUT. OPTION1 > 0 instead local and of ◦ Fix incorrect mass properties for solids in ssstat file when using *DATABASE_SSSTAT_MASS_PROPERTY. ◦ Fix seg fault during writing of dynain in *INTERFACE_SPRINGBACK in *DATABASE_EXTENT_BINARY and the *DATABASE_EXTENT_BINARY comes after *INTERFACE_SPRINGBACK. STRFLG.ne.0 INSTRN = 1 and file if ◦ If HYDRO is nonzero in *DATABASE_EXTENT_BINARY, LS-PrePost will now combine the solid and shell internal energy densities when fringing 'Internal Energy Density' in the Misc menu. ◦ By putting SIGFLG/EPSFLG = 3 in *DATABASE_EXTENT_BINARY, the stresses and plastic trains are excluded not only for shell elements but also for solids. This applies to d3plot and d3eigv. ◦ Added new file option *DATABASE_BINARY_INTFOR_FILE to define interface file name. ◦ Fixed legend in bndout in the case of multiple *BOUNDARY_PRESCRIBED_MOTION_SET_ID. ◦ Fix d3part corrupt data *DATABASE_EXTENT_BINARY. ◦ Fixed the legend of ssstat in binout. ◦ Added *DATABASE_EXTENT_SSSTAT_ID. The subsystem id will be in- DECOMP = 4 caused by in cluded in the ASCII ssstat file. ◦ Fixed bug *CONTROL_OUTPUT. in stbout (seatbelt output) if NEWLEG = 0 in ◦ Fixed bug in which DECOMP = 2 corrupted d3part. ◦ Fixed d3plot bug if dynamic relaxation was activated in the input deck. INTRODUCTION ◦ Added another digit for coordinates in *NODE in dynain, e.g., what was written as 0.999266236E+00 is now written as 9.992662368E+00. ◦ Added *DATABASE_EXTENT_BINARY_COMP for alternative (simpler) control of output to d3plot and d3eigv. Output control flags: 0-no 1-yes IGLB : Global data IXYZ : Current coordinate IVEL : Velocity IACC : Acceleration ISTRS: 6 stress data + plastic strain ISTRA: 6 strain data ISED : Strain energy density command regular This *DATABASE_EXTENT_BINARY but will disable most of the options in the latter, including output of extra history variables. combination with can be used in ◦ Bugfix: *DATABASE_TRACER without the optional NID parameter was read incorrectly when used with *INCLUDE_TRANSFORM, but is now fixed ◦ Fixed incomplete output from Windows version of LS-DYNA. This affect- curvout (*DATABASE_TRACER_DE) demtrh and ed (*DATABASE_CURVOUT). • Restarts ◦ Enable definition of sensors in full restarts. ◦ For a small restart in MPP, the value of "memory=" (M1) needed for each processor is stored in the dump files. This is the minimum requirement to read back the model info. If the value of "memory2=" (M2) is specified on the command line, the code will take the maximum of M1 and M2. input when error *INITIAL_VELOCITY_GENERATION *CHANGE_VELOCITY_GENERATION together in a full deck restart. using and structured during ◦ Fix input ◦ Fix incorrect full deck restart analysis if initial run was implicit and the full deck restart run is explicit. This affects MPP only. ◦ Fix insufficient tying of nodes when doing full deck restart and the contact is newly added to the restart involving newly added parts. This applies to SMP contact only. ◦ Fix incorrect velocity initialization for SMP full deck restart when using and *INITIAL_VELOCITY_GENERATION *INITIAL_VELOCITY_GENERATION_START_TIME. ◦ Fix incorrect initialization of velocities for SMP full deck restart when us- ing *CHANGE_VELOCITY_OPTION & *INITIAL_VELOCITY_OPTION. INTRODUCTION Velocities of existing parts defined by *STRESS_INITIALIZATION should not be zeroed. ◦ Fix *CHANGE_CURVE_DEFINITION for curve specifying d3plot output. ◦ Fixed bug in full deck restart if the new mesh has different part numbers. • *SENSOR ◦ Fix a bug for *CONSTRAINED_JOINT_STIFFNESS, that was triggered when the force refers to a local coordinate system. *SENSOR_JOINT_FORCE regarding ◦ Add the option of "ELESET" to *SENSOR_CONTROL to erode elements. ◦ Add the option of NFAILE to *SENSOR_DEFINE_MISC to track number of eroded elements. ◦ Fix a bug that was triggered when using a sensor to control spotwelds. The bug was triggered when the spotweld-connected nodal pairs happen to belong to more than 1 core (MPP only). ◦ Add FAIL option to *SENSOR_DEFINE_ELEMENT to track the failure of element(s). ◦ Fix a bug related to *SENSOR_DEFINE_FUNCTION when there are more than 10 sensor definitions. ◦ Effect of TIMEOFF TYPE = PRESC-ORI. ◦ *SENSOR_CONTROL in *SENSOR_CONTROL is implemented for can be used to control *BOUNDARY_PRESCRIBED_ORIENTATION_RIGID. ◦ Add optional filter id to SENSORD of *DEFINE_CURVE_FUNCTION. ◦ Enable *CONSTRAINED_JOINT_..._LOCAL to be monitored by *SENSOR_DEFINE_FORCE. ◦ Allow moments in SPCFORC and BNDOUT to be tracked by *SENSOR_DEFINE_FORCE. ◦ Fix *SENSOR_CONTROL using TYPE=“PRESC-MOT” which was not switching at all. • SPG (Smooth Particle Galerkin) ◦ MPP is ready in 3D SPG fluid particle stabilization (ITB = 1 & 2 in *SECTION_SOLID_SPG). ◦ Added one SPG control parameter (itb = 2) for semi-brittle fracture analy- sis. In comparison to itb = 0 or itb = 1, itb = 2 is more efficient in modeling the fragmentation and debris in semi-brittle fracture analysis such as im- pact and penetration in concrete materials. ◦ Fixed a bug related to E.O.S. in SPG. ◦ Removed some temporary memory allocations to improve efficiency. ◦ Changed the sequence of SPG initialization so that all state variables are properly initialized. INTRODUCTION ◦ Subroutines were developed for SPG failure analysis with thermal effects. Both explicit and implicit (diagonal scaled conjugate gradient iterative on- ly) SPG thermal solvers are available in SMP version only. However, thermal effect is applied only on material properties, which means thermal induced deformation (i.e., thermal strain or thermal expansion) is not cur- rently included. ◦ Modified *MAT_072R3 for SPG method in concrete applications. ◦ Fixed a bug for SPG method in using continuum damage mechanics. (ID- AM = 0). ◦ Added the “fluid particle algorithm” (itb = 1) to SPG method. This algo- rithm is implemented in R10.0 as an alternative to the (itb = 0) option in previous version to enhance the numerical stability for SPG method. Users are recommended to use this new option for their ductile failure analysis. • SPH (Smooth Particle Hydrodynamics) ◦ Add ITHK flag in *CONTROL_SPH, card 3. If flag is set to 1, the volume of the SPH particles is used to estimate a node thickness to be employed by contacts. Affects *AUTOMATIC_NODES_TO_SURFACE and *CONTACT_2D_NODE_TO_SOLID. The thickness calculated by ITHK = 1 is used only if SST or OFFD are set to zero in the contact cards definitions. ◦ Add SOFT = 1 option to *CONTACT_2D_NODE_TO_SOLID. This should help obtain reasonable contact forces in axisymmetric simulations. Default penalty PEN is 0.1 when SOFT = 1. ◦ Implemented non-reflecting boundary conditions for SPH using a new keyword *BOUNDARY_SPH_NON_REFLECTING. ◦ Bug fix for renormalized SPH formulations with symmetry planes. The renormalization was slightly incorrect in the vicinity of symmetry planes. ◦ Density smoothing in SPH formulations 15 and 16 is now material sensi- tive. The smoothing only occurs over neighbors of the same material. ◦ Resolved an MPP bug in SPH total Lagrangian formulations (FORM = 7/8) which was causing strain concentrations at the interfaces between CPU zones. ◦ SPH total Lagrangian (FORM = 7/8) in SMP was pretty much serial, hence much slower than forms 0 or 1. SPH with FORM 7 and 8 now scales properly. ◦ Added support for FORMs 0/1 in axisymmetric. Until now, renormaliza- tion was always active (equivalent to FORM = 1) which can be problematic for very large deformations or material fragmentation. ◦ Improved tracer particles output for SPH: Use normalized kernel function for interpolation between particles. INTRODUCTION ◦ Implemented enhanced fluid flow formulations (FORMs 15/16) with pres- sure smoothing. ◦ Recode SPH neighborhood search algorithm to reduce the memory re- quirement and produce consistent results from MPP and HYBRID code. ◦ *DEFINE_ADAPTIVE_SOLID_TO_SPH now reports both active and inac- tive adaptive SPH particles in the fragment file sldsph_frag. This file gives a report of nodal mass, coordinates, and velocities. ◦ MPP now supports: SPH type 3 inflow Multiple *BOUNDARY_SPH_FLOW Bulk viscosity option for SPH ◦ Sort SPH by part and then node ID to ensure consistent results while changing order of input files. ◦ *DEFINE_SPH_TO_SPH_COUPLING: Corrected the SPH sphere radius (half of the particles distance) for node to node contact detecting algorithm. Updated masses for SPH node to node coupling with damping con- tact force option. Added a new option (Soft = 1) for SPH to SPH coupling: contact stiff- ness comes from particles masses and time step for softer contact. ◦ *DEFINE_ADAPTIVE_SOLID_TO_SPH: Updated temperature transfer (from solid elements to SPH particles) when converting solid elements into SPH particles with ICPL = 1, IOPT = 0. Bug fixed when part ID for newly generated SPH particles is smaller than the original SPH part ID. Introduced a new pure thermal coupling between SPH part and solid parts with ICPL = 3 and IOPT = 0 option (no structural coupling pro- vided). Added a thermal coupling conductivity parameter CPCD. Applies to ICPL = 3 option. Normalized the nodal temperatures for the corner SPH particles with ICPL = 3 and IOPT = 0 option (MPP only). Extended ICPL = 3 and IOPT = 0 option to Lagrangian formulation (form = 7, 8). ◦ *BOUNDARY_SPH_SYMMETRY_PLANE: Added in an error message if TAIL and HEAD points are at the same location. INTRODUCTION ◦ *CONTACT_2D_NODE_TO_SOLID: Added a variable OFFD to specify contact offset. ◦ Added a new option IEROD = 2 in *CONTROL_SPH in which SPH parti- cles that satisfy a failure criterion are totally eactivated and removed from domain interpolation. This is in contrast to IEROD = 1 option in which particles are partially deactivated and only stress states are set to zero. ◦ Added *MAT_SPH_VISCOUS (*MAT_SPH_01) for fluid-like material be- havior with constant or variable viscosity. Includes a Cross viscosity mod- el. ◦ Output strain rates for SPH particles to d3plot, d3thdt, and sphout file. ◦ Added support of *MAT_ADD_EROSION, including GISSMO and DIEM damage, for SPH particles. ◦ Echo failed SPH particles into d3hsp and messag file. ◦ *DEFINE_SPH_INJECTION: Changed the method of generating SPH particles. SPH particles will be generated based on the injection volume (injection area*injection velocity*dt)*density from the material model, resulting in more con- sistent particle masses and particle distribution. Offset injecting distance inside each cycle so that outlet distance will be consistent for different outlet SPH layers. Corrected mass output in d3hsp. • Thermal Solver ◦ Modify the thermal solver routines so they return instead of terminating, so that *CASE works properly. ◦ *MAT_THERMAL_USER_DEFINED: Fixed bug in element numbering for IHVE = 1. ◦ Accept load in *CONTROL_THERMAL_TIMESTEP. As usual if a negative integer num- ber is given its absolute value refers to the load curve id. for dtmin, dtmax and dtemp curve input ◦ The temperature results for the virtual nodes of thermal thick shells are now accounted for in *LOAD_THERMAL_D3PLOT. For the mechanics- only simulation thermal thick shells have to be activated. ◦ New contact type for thermal solver that models heat transfer from and to a shell edge onto a surface (*CONTACT_..._THERMAL with ALGO > 1): Shells have to be thermal thick shells. Shells are on the slave side. So far only implemented for SMP. Includes support for quads and triangles. INTRODUCTION ◦ New keyword *BOUNDARY_THERMAL_WELD_TRAJECTORY for weld- ing of solid or shell structures. Keyword defines the movement of a heat source on a nodal path (*SET_NODE). Orientation given either by vector or with a second node set. Works for coupled and thermal only analyses. Allows for thermal dumping. Different equivalent heat source descriptions available. Can also be applied to tshells and composite shells. Weld torch motion can be defined relative to the weld trajectory. ◦ Solid element formulation 18 now supports thermal analysis. ◦ Thermal solver now supports the H8TOH20 option of *ELEMENT_SOLID. This includes support of *INITIAL_TEMPERATURE condition for the ex- tra 12 nodes generated by H8TOH20. ◦ Thermal solver now supports the H8TOH27 option of *ELEMENT_SOLID. ◦ Explicit Thermal Solver *CONTROL_EXPLICIT_THERMAL_SOLVER: Implement an explicit thermal solver and adapt it to support multi-material ALE cases. *CONTROL_EXPLICIT_THERMAL_PROPERTIES: Enter thermal properties for the explicit thermal solver. *CONTROL_EXPLICIT_THERMAL_CONTACT: Implement a ther- mal contact for the explicit thermal solver. *CONTROL_EXPLICIT_THERMAL_ALE_COUPLING: Implement a thermal coupling between ALE and Lagrangian structures for use by the explicit thermal solver. *CONSTRAINED_LAGRANGE_IN_SOLID_EDGE: For the explicit thermal ALE coupling, allow the heat transfer through the shell edges if _EDGE is added to *CONSTRAINED_LAGRANGE_IN_SOLID. *CONSTRAINED_LAGRANGE_IN_SOLID: For the explicit thermal solver, add work due to friction to the enthalpies of ALE and struc- ture with *CONSTRAINED_LAGRANGE_IN_SOLID (CTYPE = 4). elements coupled *CONTROL_EXPLICIT_THERMAL_INITIAL: Initialize the tempera- tures for the explicit thermal solver. *CONTROL_EXPLICIT_THERMAL_BOUNDARY: Control boundary temperatures for the explicit thermal solver. *CONTROL_EXPLICIT_THERMAL_OUTPUT: Output the tempera- tures at element centers for the explicit thermal solver. *DATABASE_PROFILE: For the explicit thermal solver, output tem- perature profiles. • Miscellaneous INTRODUCTION ◦ *INITIAL_LAG_MAPPING: Implement a 3D to 3D lagrangian mapping and map the nodal temperatures. ◦ *CONTROL_REFINE_SHELL and *CONTROL_REFINE_SOLID: Add a parameter MASTERSET to call a set of nodes to flag element edges along which new child nodes are constrained. ◦ *BOUNDARY_PRESCRIBED_MOTION_SET_SEGMENT: Add DOF = 12 to apply velocities in local coordinate systems attached to segments. ◦ Fixed bug when occurring non-zero *DAMPING_PART_STIFFNESS, using *PART_COMPOSITE, AND the MIDs referenced by the different integra- tion points have different material types. Symptoms could include many types of unexpected behavior or error termination, but in other cases it could be harmless. has defined a AND part is ◦ *DAMPING_FREQUENCY_RANGE (including _DEFORM option): Im- proved internal calculation of damping constants such that the level of damping more accurately matches the user-input value across the whole of the frequency range FLOW to FHIGH. As an example, for CDAMP = 0.01, FLOW = 1 Hz and FHIGH = 30 Hz, the actual damping achieved by the previous algorithm varied between 0.008 and 0.012 (different values at dif- ferent frequencies between FLOW and FHIGH), i.e. there were errors of up to 20% of the target CDAMP. With the new algorithm, the errors are reduced to 1% of the target CDAMP. This change will lead to some small differences in results compared to previous versions of LS-DYNA. Users wishing to retain the old method for compatibility with previous work can do this by setting IFLG (7th field on Card 1) to 1. in the Part included ◦ Fixed bug that could cause unpredictable symptoms if Nodal Rigid Bodies by were or *DAMPING_FREQUENCY_RANGE *DAMPING_FREQUENCY_RANGE_DEFORM. Now, the _DEFORM op- tion Set while *DAMPING_FREQUENCY_RANGE (non _DEFORM option) damps them. ◦ Fixed bug in *PART_COMPOSITE: if a layer had a very small thickness de- fined, such as 1E-9 times the total thickness, that layer would be assigned a weighting factor of 1 (it should be close to zero). ignores NRBs referenced silently Part the Set in ◦ Fix errors in implementation of *DEFINE_FILTER type CHAIN. ◦ Fix for *INTERFACE_LINKING_LOCAL when LCID is used. During keyword processing, the LCID value was not properly converted to inter- nal numbering. ◦ Switch coordinates in keyword reader to double precision. ◦ Change "Warning" to "Error" for multiply defined materials, boxes, coordi- nate systems, vectors, and orientation vectors. The check for duplicate sec- tion IDs now includes the element type and remains a warning for now, because SPH is still detected as a SOLID. Once that is straightened out, this should be made an error. INTRODUCTION ◦ Add "TIMESTEP" as a variable for *DEFINE_CURVE_FUNCTION. This variable holds the current simulation time step. ◦ Fix a bug in *DEFORMABLE_TO_RIGID_AUTOMATIC. (Fields 3 to 8 are now ig- nored.) CODE = 5 case the for of ◦ Issue error message and terminate the simulation when illegal ACTION is used for *DEFINE_TRANSFORM. ◦ Add option of POS6N for *DEFINE_TRANSFORM to define transfor- mation with 3 reference nodes and 3 target nodes. ◦ Fix a bug that can occur when adaptive elements are defined in a file in- cluded by *INCLUDE_TRANSFORM. ◦ Merge *DEFORMABLE_TO_RIGID_AUTOMATIC cards if they use the same switch time. This dependency of results on the order of the cards and also gives better performance. ◦ If *SET_PART_OPTION is used, a "group_file" will be created which can be read into LS-Prepost (Model > Groups > Load) for easy visualization of part sets. ◦ Forces on *RIGIDWALL_GEOMETRIC_CYLINDER can now be subdivid- ed into sections for output to rwforc. This gives a better idea of the force distribution along the length of the cylinder. See the variable NSEGS. ◦ Added the keywords *DEFINE_PRESSURE_TUBE and *DATABASE_PRTUBE for simulating pressure tubes in pedestrian crash. ◦ Fix non-effective OPTIONs DBOX, DVOL, DSOLID, DSHELL, DTSHELL, DSEG for *SET_SEGMENT_GENERAL to delete segments. ◦ Fix incorrect transformation of valdmp in *DAMPING_GLOBAL with *INCLUDE_TRANSFORM. ◦ Make *SET_NODE_COLLECT work together with *NODE_SET_MERGE. ◦ Fixed bug in adaptivity for *INCLUDE_TRANSFORM if jobid is used. ◦ Bugfix: *INTERFACE_SSI with blank optional card is now read in correct- ly. MATERIAL MODELS Some of the material models presently implemented are: • elastic, • orthotropic elastic, • kinematic/isotropic plasticity [Krieg and Key 1976], • thermoelastoplastic [Hallquist 1979], • soil and crushable/non-crushable foam [Key 1974], • linear viscoelastic [Key 1974], INTRODUCTION • Blatz-Ko rubber [Key 1974], • high explosive burn, • hydrodynamic without deviatoric stresses, • elastoplastic hydrodynamic, • temperature dependent elastoplastic [Steinberg and Guinan 1978], • isotropic elastoplastic, • isotropic elastoplastic with failure, • soil and crushable foam with failure, • Johnson/Cook plasticity model [Johnson and Cook 1983], • pseudo TENSOR geological model [Sackett 1987], • elastoplastic with fracture, • power law isotropic plasticity, • strain rate dependent plasticity, • rigid, • thermal orthotropic, • composite damage model [Chang and Chang 1987a 1987b], • thermal orthotropic with 12 curves, • piecewise linear isotropic plasticity, • inviscid, two invariant geologic cap [Sandler and Rubin 1979, Simo et al, 1988a • 1988b], • orthotropic crushable model, • Mooney-Rivlin rubber, • resultant plasticity, • force limited resultant formulation, • closed form update shell plasticity, • Frazer-Nash rubber model, • laminated glass model, • fabric, • unified creep plasticity, • temperature and rate dependent plasticity, • elastic with viscosity, • anisotropic plasticity, INTRODUCTION • user defined, • crushable cellular foams [Neilsen, Morgan, and Krieg 1987], • urethane foam model with hysteresis, and some more foam and rubber models, as well as many materials models for springs and dampers. The hydrodynamic material models determine only the deviatoric stresses. Pressure is determined by one of ten equations of state including: • linear polynomial [Woodruff 1973], • JWL high explosive [Dobratz 1981], • Sack “Tuesday” high explosive [Woodruff 1973], • Gruneisen [Woodruff 1973], • ratio of polynomials [Woodruff 1973], • linear polynomial with energy deposition, • ignition and growth of reaction in HE [Lee and Tarver 1980, Cochran and Chan 1979], • tabulated compaction, • tabulated, • TENSOR pore collapse [Burton et al. 1982]. The ignition and growth EOS was adapted from KOVEC [Woodruff 1973]; the other subroutines, programmed by the authors, are based in part on the cited references and are nearly 100 percent vectorized. The forms of the first five equations of state are also given in the KOVEC user’s manual and are retained in this manual. The high explosive programmed burn model is described by Giroux [Simo et al. 1988]. The orthotropic elastic and the rubber material subroutines use Green-St. Venant strains to compute second Piola-Kirchhoff stresses, which transform to Cauchy stresses. The Jaumann stress rate formulation is used with all other materials with the exception of one plasticity model which uses the Green-Naghdi rate. SPATIAL DISCRETIZATION are presently available. Currently springs, dampers, beams, membranes, shells, bricks, thick shells and seatbelt elements are included. The first shell element in DYNA3D was that of Hughes and Liu [Hughes and Liu 1981a, 1981b, 1981c], implemented as described in [Hallquist et al. 1985, Hallquist and Benson 1986]. This element [designated as HL] was selected from among a substantial body of shell element literature because the element formulation has several desirable qualities: INTRODUCTION Shells Solids Beams Trusses Springs Lumped Masses Damper Elements in LS-DYNA. Figure 1-1. Three-dimensional plane stress constitutive subroutines are implemented for the shell elements which iteratively update the stress tensor such that the stress component normal to the shell midsurface is zero. An iterative update is necessary to accurately determine the normal strain component which is necessary to predict thinning. One constitutive evaluation is made for each integration point through the h ll thi k • It is incrementally objective (rigid body rotations do not generate strains), allowing for the treatment of finite strains that occur in many practical applica- tions. • It is compatible with brick elements, because the element is based on a degener- ated brick element formulation. This compatibility allows many of the efficient and effective techniques developed for the DYNA3D brick elements to be used with this shell element; • It includes finite transverse shear strains; • A through-the-thickness thinning option is also available. All shells in our current LS-DYNA code must satisfy these desirable traits to at least some extent to be useful in metalforming and crash simulations. The major disadvantage of the HL element turned out to be cost related and, for this reason, within a year of its implementation we looked at the Belytschko-Tsay [BT] shell [Belytschko and Tsay 1981, 1983, 1984] as a more cost effective, but possibly less accurate alternative. In the BT shell the geometry of the shell is assumed to be perfectly flat, the local coordinate system originates at the first node of the connectivity, and the INTRODUCTION co-rotational stress update does not use the costly Jaumann stress rotation. With these and other simplifications, a very cost effective shell was derived which today has become perhaps the most widely used shell elements in both metalforming and crash applications. Results generated by the BT shell usually compare favorably with those of the more costly HL shell. Triangular shell elements are implemented, based on work by Belytschko and co-workers [Belytschko and Marchertas 1974, Bazeley et al. 1965, Belytschko et al. 1984], and are frequently used since collapsed quadrilateral shell elements tend to lock and give very bad results. LS-DYNA automatically treats collapsed quadrilateral shell elements as C0 triangular elements. Since the Belytschko-Tsay element is based on a perfectly flat geometry, warpage is not considered. Although this generally poses no major difficulties and provides for an efficient element, incorrect results in the twisted beam problem and similar situations are obtained where the nodal points of the elements used in the discretization are not coplanar. The Hughes-Liu shell element considers non-planar geometries and gives good results on the twisted beam. The effect of neglecting warpage in a typical application cannot be predicted beforehand and may lead to less than accurate results, but the latter is only speculation and is difficult to verify in practice. Obviously, it would be better to use shells that consider warpage if the added costs are reasonable and if this unknown effect is eliminated. Another shell published by Belytschko, Wong, and Chiang [Belytschko, Wong, and Chiang 1989, 1992] proposes inexpensive modifications to include the warping stiffness in the Belytschko-Tsay shell. An improved transverse shear treatment also allows the element to pass the Kirchhoff patch test. This element is now available in LS-DYNA. Also, two fully integrated shell elements, based on the Hughes and Liu formulation, are available in LS-DYNA, but are rather expensive. A much faster fully integrated element which is essentially a fully integrated version of the Belytschko, Wong, and Chiang element, type 16, is a more recent addition and is recommended if fully integrated elements are needed due to its cost effectiveness. Zero energy modes in the shell and solid elements are controlled by either an hourglass viscosity or stiffness. Eight node thick shell elements are implemented and have been found to perform well in many applications. All elements are nearly 100% vectorized. All element classes can be included as parts of a rigid body. The rigid body formulation is documented in [Benson and Hallquist 1986]. Rigid body point nodes, as well as concentrated masses, springs and dashpots can be added to this rigid body. Membrane elements can be either defined directly as shell elements with a membrane formulation option or as shell elements with only one point for through thickness integration. The latter choice includes transverse shear stiffness and may be inappropriate. For airbag material a special fully integrated three and four node membrane element is available. INTRODUCTION Two different beam types are available: a stress resultant beam and a beam with cross section integration at one point along the axis. The cross section integration allows for a more general definition of arbitrarily shaped cross sections taking into account material nonlinearities. Spring and damper elements can be translational or rotational. Many behavior options can be defined, e.g., arbitrary nonlinear behavior including locking and separation. Solid elements in LS-DYNA may be defined using from 4 to 8 nodes. The standard elements are based on linear shape functions and use one point integration and hourglass control. A selective-reduced integrated (called fully integrated) 8 node solid element is available for situations when the hourglass control fails. Also, two additional solid elements, a 4 noded tetrahedron and an 8 noded hexahedron, with nodal rotational degrees of freedom, are implemented based on the idea of Allman [1984] to replace the nodal midside translational degrees of freedom of the elements with quadratic shape functions by corresponding nodal rotations at the corner nodes. The latter elements, which do not need hourglass control, require many numerical operations compared to the hourglass controlled elements and should be used at places where the hourglass elements fail. However, it is well known that the elements using more than one point integration are more sensitive to large distortions than one point integrated elements. The thick shell element is a shell element with only nodal translations for the eight nodes. The assumptions of shell theory are included in a non-standard fashion. It also uses hourglass control or selective-reduced integration. This element can be used in place of any four node shell element. It is favorably used for shell-brick transitions, as no additional constraint conditions are necessary. However, care has to be taken to know in which direction the shell assumptions are made; therefore, the numbering of the element is important. Seatbelt elements can be separately defined to model seatbelt actions combined with dummy models. Separate definitions of seatbelts, which are one-dimensional elements, with accelerometers, sensors, pretensioners, retractors, and sliprings are possible. The actions of the various seatbelt definitions can also be arbitrarily combined. CONTACT-IMPACT INTERFACES The three-dimensional contact-impact algorithm was originally an extension of the NIKE2D [Hallquist 1979] two-dimensional algorithm. As currently implemented, one surface of the interface is identified as a master surface and the other as a slave. Each surface is defined by a set of three or four node quadrilateral segments, called master and slave segments, on which the nodes of the slave and master surfaces, respectively, must slide. In general, an input for the contact-impact algorithm requires that a list of INTRODUCTION master and slave segments be defined. For the single surface algorithm only the slave surface is defined and each node in the surface is checked each time step to ensure that it does not penetrate through the surface. Internal logic [Hallquist 1977, Hallquist et al. 1985] identifies a master segment for each slave node and a slave segment for each master node and updates this information every time step as the slave and master nodes slide along their respective surfaces. It must be noted that for general automatic definitions only parts/materials or three-dimensional boxes have to be given. Then the possible contacting outer surfaces are identified by the internal logic in LS-DYNA. More than 20 types of interfaces can presently be defined including: •sliding only for fluid/structure or gas/structure interfaces •tied •sliding, impact, friction •single surface contact •discrete nodes impacting surface •discrete nodes tied to surface •shell edge tied to shell surface •nodes spot welded to surface •tiebreak interface •one way treatment of sliding, impact, friction •box/material limited automatic contact for shells •automatic contact for shells (no additional input required) •automatic single surface with beams and arbitrary orientations •surface to surface eroding contact •node to surface eroding contact •single surface eroding contact •surface to surface symmetric constraint method [Taylor and Flanagan 1989] •node to surface constraint method [Taylor and Flanagan 1989] •rigid body to rigid body contact with arbitrary force/deflection curve •rigid nodes to rigid body contact with arbitrary force/deflection curve •edge-to-edge •draw beads Interface friction can be used with most interface types. The tied and sliding only interface options are similar to the two-dimensional algorithm used in LS-DYNA2D [Hallquist 1976, 1978, 1980]. Unlike the general option, the tied treatments are not symmetric; therefore, the surface which is more coarsely zoned should be chosen as the master surface. When using the one-way slide surface with rigid materials, the rigid material should be chosen as the master surface. For geometric contact entities, contact has to be separately defined. It must be noted that for the contact of a rigid body with a flexible body, either the sliding interface definitions as explained above or the geometric contact entity contact can be used. INTRODUCTION Currently, the geometric contact entity definition is recommended for metalforming problems due to high accuracy and computational efficiency. INTERFACE DEFINITIONS FOR COMPONENT ANALYSIS Interface definitions for component analyses are used to define surfaces, nodal lines, or nodal points (*INTERFACE_COMPONENTS) for which the displacement and velocity time histories are saved at some user specified frequency (*CONTROL_OUTPUT). This data may then used to drive interfaces (*INTERFACE_LINKING) in subsequent analyses. This capability is especially useful for studying the detailed response of a small member in a large structure. For the first analysis, the member of interest need only be discretized sufficiently that the displacements and velocities on its boundaries are reasonably accurate. After the first analysis is completed, the member can be finely discretized and interfaces defined to correspond with the first analysis. Finally, the second analysis is performed to obtain highly detailed information in the local region of interest. When starting the analysis, specify a name for the interface segment file using the Z = parameter on the LS-DYNA command line. When starting the second analysis, the name of the interface segment file (created in the first run) should be specified using the L = parameter on the LS-DYNA command line. the above procedure, multiple levels of sub-modeling are easily Following accommodated. The interface file may contain a multitude of interface definitions so that a single run of a full model can provide enough interface data for many component analyses. The interface feature represents a powerful extension of LS-DYNA’s analysis capability. PRECISION to machine precision The explicit time integration algorithms used in LS-DYNA are in general much less sensitive finite element solution methods. than other Consequently, double precision is not generally required. The benefits of this are greatly improved utilization of memory and disk. When problems have been found we have usually been able to overcome them by reorganizing the algorithm or by converting to double precision locally in the subroutine where the problem occurs. Particularly sensitive problems (e.g. some buckling problems, which can be sensitive to small imperfections) may require the fully double precision version, which is available on all platforms. Very large problems requiring more than 2 billion words of memory will also need to be run in double precision, due to the array indexing limitation of single precision integers. Getting Started GETTING STARTED DESCRIPTION OF KEYWORD INPUT The keyword input provides a flexible and logically organized database that is simple to understand. Similar functions are grouped together under the same keyword. For example, under the keyword *ELEMENT are included solid, beam, shell elements, spring elements, discrete dampers, seat belts, and lumped masses. Many keywords have options that are identified as follows: “OPTIONS” and “{OPTIONS}”. The difference is that “OPTIONS” requires that one of the options must be selected to complete the keyword command. The option <BLANK> is included when {} are used to further indicate that these particular options are not necessary to complete the keyword. LS-DYNA User’s Manual is alphabetically organized in logical sections of input data. Each logical section relates to a particular input. There is a control section for resetting LS-DYNA defaults, a material section for defining constitutive constants, an equation- of-state section, an element section where element part identifiers and nodal connectivities are defined, a section for defining parts, and so on. Nearly all model data can be input in block form. For example, consider the following where two nodal points with their respective coordinates and shell elements with their part identity and nodal connectivity’s are defined: $define two nodes $ *NODE 10101x y z 10201x y z $ define two shell elements $ *ELEMENT_SHELL 10201pidn1n2n3n4 10301pidn1n2n3n4 Alternatively, acceptable input could also be of the form: $ define one node $ *NODE 10101x y z $ define one shell element $ *ELEMENT_SHELL 10201pidn1n2n3n4 $ $ define one more node $ *NODE 10201x y z $ define one more shell element $ *ELEMENT_SHELL 10301pidn1n2n3n4 Getting Started *NODE *ELEMENT *PART NID X Y Z EID PID N1 N2 N3 N4 PID SID MID EOSID HGID *SECTION_SHELL SID ELFORM SHRF NIP PROPT QR ICOMP *MAT_ELASTIC MID RO E PR DA DB *EOS *HOURGLASS EOSID HGID Figure 2-1. Organization of the keyword input. A data block begins with a keyword followed by the data pertaining to the keyword. The next keyword encountered during the reading of the block data defines the end of the block and the beginning of a new block. A keyword must be left justified with the “*” contained in column one. A dollar sign “$” in column one precedes a comment and causes the input line to be ignored. Data blocks are not a requirement for LS-DYNA but they can be used to group nodes and elements for user convenience. Multiple blocks can be defined with each keyword if desired as shown above. It would be possible to put all nodal points definitions under one keyword *NODE, or to define one *NODE keyword prior to each node definition. The entire LS-DYNA input is order independent with the exception of the optional keyword, *END, which defines the end of input stream. Without the *END termination is assumed to occur when an end-of- file is encountered during the reading. Figure 2-1 highlights how various entities relate to each other in LS-DYNA input. In this figure the data included for the keyword, *ELEMENT, is the element identifier, EID, the part identifier, PID, and the nodal points identifiers, the NID’s, defining the element connectivity: N1, N2, N3, and N4. The nodal point identifiers are defined in the *NODE section where each NID should be defined just once. A part defined with the *PART keyword has a unique part identifier, PID, a section identifier, SID, a material or constitutive model identifier, MID, an equation of state identifier, EOSID, and the hourglass control identifier, HGID. The *SECTION keyword defines the section identifier, SID, where a section has an element formulation specified, a shear factor, SHRF, a numerical integration rule, NIP, among other parameters. Constitutive constants are defined in the *MAT section where constitutive data is defined for all element types including solids, beams, shells, thick shells, seat belts, springs, and dampers. Equations of state, which are used only with certain *MAT materials for solid elements, are defined in the *EOS section. Since many elements in LS-DYNA use uniformly reduced numerical integration, zero energy deformation modes may develop. These modes are controlled numerically by either an artificial stiffness or viscosity which resists the formation of these undesirable modes. The hourglass control can optionally be user specified using the input in the *HOURGLASS section. Getting Started During the keyword input phase where data is read, only limited checking is performed on the data since the data must first be counted for the array allocations and then reordered. Considerably more checking is done during the second phase where the input data is printed out. Since LS-DYNA has retained the option of reading older non- keyword input files, we print out the data into the output file d3hsp (default name) as in previous versions of LS-DYNA. An attempt is made to complete the input phase before error terminating if errors are encountered in the input. Unfortunately, this is not always possible and the code may terminate with an error message. The user should always check either output file, d3hsp or messag, for the word “Error”. The input data following each keyword can be input in free format. In the case of free format input the data is separated by commas, i.e., *NODE 10101,x ,y ,z 10201,x ,y ,z *ELEMENT_SHELL 10201,pid,n1,n2,n3,n4 10301,pid,n1,n2,n3,n4 When using commas, the formats must not be violated. An I8 integer is limited to a maximum positive value of 99999999, and larger numbers having more than eight characters are unacceptable. The format of the input can change from free to fixed anywhere in the input file. The input is case insensitive and keywords can be given in either upper or lower case. The asterisks “*” preceding each keyword must be in column one. To provide a better understanding behind the keyword philosophy and how the options work, a brief review the keywords is given below. *AIRBAG The geometric definition of airbags and the thermodynamic properties for the airbag inflator models can be made in this section. This capability is not necessarily limited to the modeling of automotive airbags, but it can also be used for many other applications such as tires and pneumatic dampers. *ALE This keyword provides a way of defining input data pertaining to the Arbitrary- Lagrangian-Eulerian capability. This section applies to various methods of specifying either fixed or prescribed boundary conditions. For compatibility with older versions of LS-DYNA it is still possible to specify some nodal boundary conditions in the *NODE card section. *CASE This keyword option provides a way of running multiple load cases sequentially. Within each case, the input parameters, which include loads, boundary conditions, control cards, contact definitions, initial conditions, etc., can change. If desired, the results from a previous case can be used during initialization. Each case creates unique file names for all output results files by appending CIDn to the default file name. *COMPONENT This section contains analytical rigid body dummies that can be placed within vehicle and integrated implicitly. *CONSTRAINED This section applies constraints within the structure between structural parts. For example, nodal rigid bodies, rivets, spot welds, linear constraints, tying a shell edge to a shell edge with failure, merging rigid bodies, adding extra nodes to rigid bodies and defining rigid body joints are all options in this section. *CONTACT This section is divided in to three main sections. The *CONTACT section allows the user to define many different contact types. These contact options are primarily for treating contact of deformable to deformable bodies, single surface contact in deformable bodies, deformable body to rigid body contact, and tying deformable structures with an option to release the tie based on plastic strain. The surface definition for contact is made up of segments on the shell or solid element surfaces. The keyword options and the corresponding numbers in previous code versions are: STRUCTURED INPUT TYPE ID KEYWORD NAME 1 p 1 2 SLIDING_ONLY SLIDING_ONLY_PENALTY TIED_SURFACE_TO_SURFACE 3 a 3 4 5 a 5 6 7 8 9 10 a 10 13 a 13 14 15 16 17 18 19 20 21 22 23 Getting Started SURFACE_TO_SURFACE AUTOMATIC_SURFACE_TO_SURFACE SINGLE_SURFACE NODES_TO_SURFACE AUTOMATIC_NODES_TO_SURFACE TIED_NODES_TO_SURFACE TIED_SHELL_EDGE_TO_SURFACE TIEBREAK_NODES_TO_SURFACE TIEBREAK_SURFACE_TO_SURFACE ONE_WAY_SURFACE_TO_SURFACE AUTOMATIC_ONE_WAY_SURFACE_TO_SURFACE AUTOMATIC_SINGLE_SURFACE AIRBAG_SINGLE_SURFACE ERODING_SURFACE_TO_SURFACE ERODING_SINGLE_SURFACE ERODING_NODES_TO_SURFACE CONSTRAINT_SURFACE_TO_SURFACE CONSTRAINT_NODES_TO_SURFACE RIGID_BODY_TWO_WAY_TO_RIGID_BODY RIGID_NODES_TO_RIGID_BODY RIGID_BODY_ONE_WAY_TO_RIGID_BODY SINGLE_EDGE DRAWBEAD Getting Started The *CONTACT_ENTITY section treats contact between a rigid surface, usually defined as an analytical surface, and a deformable structure. Applications of this type of contact exist in the metal forming area where the punch and die surface geometries can be input as VDA surfaces which are treated as rigid. Another application is treating contact between rigid body occupant dummy hyper-ellipsoids and deformable structures such as airbags and instrument panels. This option is particularly valuable in coupling with the rigid body occupant modeling codes MADYMO and CAL3D. The *CONTACT_1D is for modeling rebars in concrete structure. *CONTROL Options available in the *CONTROL section allow the resetting of default global parameters such as the hourglass type, the contact penalty scale factor, shell element formulation, numerical damping, and termination time. *DAMPING Defines damping either globally or by part identifier. *DATABASE This keyword with a combination of options can be used for controlling the output of ASCII databases and binary files output by LS-DYNA. With this keyword the frequency of writing the various databases can be determined. *DEFINE This section allows the user to define curves for loading, constitutive behaviors, etc.; boxes to limit the geometric extent of certain inputs; local coordinate systems; vectors; and orientation vectors specific to spring and damper elements. Items defined in this section are referenced by their identifiers throughout the input. For example, a coordinate system identifier is sometimes used on the *BOUNDARY cards, and load curves are used on the *AIRBAG cards. *DEFORMABLE_TO_RIGID This section allows the user to switch parts that are defined as deformable to rigid at the start of the analysis. This capability provides a cost efficient method for simulating events such as rollover events. While the vehicle is rotating the computation cost can be reduced significantly by switching deformable parts that are not expected to deform to rigid parts. Just before the vehicle comes in contact with ground, the analysis can be stopped and restarted with the part switched back to deformable. Define identifiers and connectivities for all elements which include shells, beams, solids, thick shells, springs, dampers, seat belts, and concentrated masses in LS-DYNA. *EOS This section reads the equations of state parameters. The equation of state identifier, EOSID, points to the equation of state identifier on the *PART card. *HOURGLASS Defines hourglass and bulk viscosity properties. The identifier, HGID, on the *HOURGLASS card refers to HGID on *PART card. *INCLUDE To make the input file easy to maintain, this keyword allows the input file to be split into sub-files. Each sub-file can again be split into sub-sub-files and so on. This option is beneficial when the input data deck is very large. *INITIAL Initial velocity and initial momentum for the structure can be specified in this section. The initial velocity specification can be made by *INITIAL_VELOCITY_NODE card or *INITIAL_VELOCITY cards. In the case of *INITIAL_VELOCITY_NODE nodal identifiers are used to specify the velocity components for the node. Since all the nodes in the system are initialized to zero, only the nodes with non-zero velocities need to be specified. The *INITIAL_VELOCITY card provides the capability of being able to specify velocities using the set concept or boxes. *INTEGRATION In this section the user defined integration rules for beam and shell elements are specified. IRID refers to integration rule number IRID on *SECTION_BEAM and *SEC- TION_SHELL cards respectively. Quadrature rules in the *SECTION_SHELL and *SECTION_BEAM cards need to be specified as a negative number. The absolute value of the negative number refers to user defined integration rule number. Positive rule numbers refer to the built in quadrature rules within LS-DYNA. Interface definitions are used to define surfaces, nodal lines, and nodal points for which the displacement and velocity time histories are saved at some user specified frequency. This data may then be used in subsequent analyses as an interface ID in the *INTER- FACE_LINKING_DISCRETE_NODE as master nodes, in *INTERFACE_LINKING_- SEGMENT as master segments and in *INTERFACE_LINKING_EDGE as the master edge for a series of nodes. This capability is especially useful for studying the detailed response of a small member in a large structure. For the first analysis, the member of interest need only be discretized sufficiently that the displacements and velocities on its boundaries are reasonably accurate. After the first analysis is completed, the member can be finely discretized in the region bounded by the interfaces. Finally, the second analysis is performed to obtain highly detailed information in the local region of interest. When beginning the first analysis, specify a name for the interface segment file using the Z=parameter on the LS-DYNA execution line. When starting the second analysis, the name of the interface segment file created in the first run should be specified using the L=parameter on the LS-DYNA command line. Following the above procedure, multiple levels of sub-modeling are easily accommodated. The interface file may contain a multitude of interface definitions so that a single run of a full model can provide enough interface data for many component analyses. The interface feature represents a powerful extension of LS-DYNA’s analysis capabilities. A similar capability using *INTERFACE_SSI may be used for soil-structure interaction analysis under earthquake excitation. *KEYWORD Flags LS-DYNA that the input deck is a keyword deck. To have an effect this must be the very first card in the input deck. Alternatively, by typing “keyword” on the execute line, keyword input formats are assumed and the “*KEYWORD” is not required. If a number is specified on this card after the word KEYWORD it defines the memory size to used in words. The memory size can also be set on the command line. NOTE: The memory specified on the execution line over- rides memory specified on the *keyword card. *LOAD This section provides various methods of loading the structure with concentrated point loads, distributed pressures, body force loads, and a variety of thermal loadings. This section allows the definition of constitutive constants for all material models available in LS-DYNA including springs, dampers, and seat belts. The material identifier, MID, points to the MID on the *PART card. *NODE Define nodal point identifiers and their coordinates. *PARAMETER This option provides a way of specifying numerical values of parameter names that are referenced throughout the input file. The parameter definitions, if used, should be placed at the beginning of the input file following *KEYWORD. *PARAMETER_EX- PRESSION permits general algebraic expressions to be used to set the values. *PART This keyword serves two purposes. 1. Relates part ID to *SECTION, *MATERIAL, *EOS and *HOURGLASS sections. 2. Optionally, in the case of a rigid material, rigid body inertia properties and initial conditions can be specified. Deformable material repositioning data can also be specified in this section if the reposition option is invoked on the *PART card, i.e., *PART_REPOSITION. *PERTURBATION This keyword provides a way of defining deviations from the designed structure such as, buckling imperfections. *RAIL This keyword provides a way of defining a wheel-rail contact algorithm intended for railway applications but can also be used for other purposes. The wheel nodes (defined on *RAIL_TRAIN) represent the contact patch between wheel and rail. *RIGIDWALL Rigid wall definitions have been divided into two separate sections, PLANAR and GEOMETRIC. Planar walls can be either stationary or moving in translational motion Getting Started with mass and initial velocity. The planar wall can be either finite or infinite. Geometric walls can be planar as well as have the geometric shapes such as rectangular prism, cylindrical prism and sphere. By default, these walls are stationary unless the option MOTION is invoked for either prescribed translational velocity or displacement. Unlike the planar walls, the motion of the geometric wall is governed by a load curve. Multiple geometric walls can be defined to model combinations of geometric shapes available. For example, a wall defined with the CYLINDER option can be combined with two walls defined with the SPHERICAL option to model hemispherical surface caps on the two ends of a cylinder. Contact entities are also analytical surfaces but have the significant advantage that the motion can be influenced by the contact to other bodies, or prescribed with six full degrees-of-freedom. *SECTION In this section, the element formulation, integration rule, nodal thicknesses, and cross sectional properties are defined. All section identifiers (SECID’s) defined in this section must be unique, i.e., if a number is used as a section ID for a beam element then this number cannot be used again as a section ID for a solid element. *SENSOR This keyword provides a convenient way of activating and deactivating boundary conditions, airbags, discrete elements, joints, contact, rigid walls, single point constraints, and constrained nodes. The sensor capability is new in the second release of version 971 and will evolve in later releases to encompass many more LS-DYNA capabilities and replace some of the existing capabilities such as the airbag sensor logic. *SET A concept of grouping nodes, elements, materials, etc., in sets is employed throughout the LS-DYNA input deck. Sets of data entities can be used for output. So-called slave nodes used in contact definitions, slaves segment sets, master segment sets, pressure segment sets and so on can also be defined. The keyword, *SET, can be defined in two ways: 1. Option LIST requires a list of entities, eight entities per card, and define as many cards as needed to define all the entities. 2. Option COLUMN, where applicable, requires an input of one entity per line along with up to four attribute values which are used by other keywords to specify, for example, the failure criterion input that is needed for *CONTACT_- CONSTRAINT_NODES_TO_SURFACE. This keyword provides an alternative way of stopping the calculation before the termination time is reached. The termination time is specified on the *CONTROL_TER- MINATION input and will terminate the calculation whether or not the options available in this section are active. *TITLE In this section a title for the analysis is defined. *USER_INTERFACE This section provides a method to provide user control of some aspects of the contact algorithms including friction coefficients via user defined subroutines. RESTART This section of the input is intended to allow the user to restart the simulation by providing a restart file and optionally a restart input defining changes to the model such as deleting contacts, materials, elements, switching materials from rigid to deformable, deformable to rigid, etc. *RIGID_DEFORMABLE This section switches rigid parts back to deformable in a restart to continue the event of a part impacting the ground which may have been modeled with a rigid wall. *STRESS_INITIALIZATION This is an option available for restart runs. In some cases there may be a need for the user to add contacts, elements, etc., which are not available options for standard restart runs. A full input containing the additions is needed if this option is invoked upon restart. Getting Started SUMMARY OF COMMONLY USED OPTIONS The following table gives a list of the commonly used keywords related by topic. Topic Component Keywords Nodes Elements Geometry Discrete Elements Part Material Materials Sections Discrete sections *NODE *ELEMENT_BEAM *ELEMENT_SHELL *ELEMENT_SOLID *ELEMENT_TSHELL *ELEMENT_DISCRETE *ELEMENT_SEATBELT *ELEMENT_MASS PART cards glues the model together: ⎧*MAT {{ *SECTION {{⎨ *EOS ⎩ *HOURGLASS *PART → *MAT *SECTION_BEAM *SECTION_SHELL *SECTION_SOLID *SECTION_TSHELL *SECTION_DISCRETE *SECTION_SEATBELT Equation of state *EOS Hourglass Contacts & Rigid walls Defaults for contacts Definition of contacts Definition of rigid walls *CONTROL_HOURGLASS *HOURGLASS *CONTROL_CONTACT *CONTACT_OPTION *RIGIDWALL_OPTION Topic Component Keywords Getting Started Boundary Conditions & Loadings Constraints and spot welds Output Control Restraints Gravity (body) load Point load Pressure load Thermal load Load curves Constrained nodes Welds Rivet *NODE *BOUNDARY_SPC_OPTION *LOAD_BODY_OPTION *LOAD_NODE_OPTION *LOAD_SEGMENT_OPTION *LOAD_SHELL_OPTION *LOAD_THERMAL_OPTION *DEFINE_CURVE *CONSTRAINED_NODE_SET *CONSTRAINED_GENERALIZED_WELD *CONSTRAINED_SPOT_WELD *CONSTRAINED_RIVET Items in time history blocks *DATABASE_HISTORY_OPTION Default ASCII time history files *CONTROL_OUTPUT *DATABASE_OPTION Binary plot/time history/restart files *DATABASE_BINARY_OPTION Nodal reaction output *DATABASE_NODAL_FORCE_GROUP Termination Termination time Termination cycle CPU termination Degree of freedom *CONTROL_TERMINATION *CONTROL_TERMINATION *CONTROL_CPU *TERMINATION_NODE Table 2.1. Keywords for the most commonly used options. EXECUTION SYNTAX The execution line for LS-DYNA, sometimes referred to as the command line, is as follows: Getting Started LS-DYNA I=inf O=otf G=ptf D3PART=d3part D=dpf F=thf T=tpf A=rrd M=sif S=iff H=iff Z=isf1 L=isf2 B=rlf W=root E=efl X=scl C=cpu K=kill V=vda Y=c3d BEM=bof {KEYWORD} {THERMAL} {COUPLE} {INIT} {CASE} {PGPKEY} MEMORY=nwds MODULE=dll NCPU=ncpu PA- RA=para JOBID=jobid D3PROP=d3prop GMINP=gminp GMOUT=gmout MCHECK=y NCYCLE=ncycle ENDTIME=time where, inf = input file (user specified) otf = high speed printer file (default = d3hsp) ptf = binary plot file for postprocessing (default = d3plot) d3part = binary plot file for subset of parts; see *DATABASE_BINARY_D3PART (default = d3part) dpf = dump file to write for purposes of restarting (default = d3dump). This file is written at the end of every run and during the run as requested by *DATABASE_BINARY_D3DUMP. To stop the generation of this dump file, specify “d=nodump” (case insensitive). thf = binary plot file for time histories of selected data (default = d3thdt) tpf = optional temperature file rrd = running restart dump file (default = runrsf) sif = stress initialization file (user specified) iff = interface force file (user specified). See *DATBASE_BINARY_INTFOR and *DATABASE_BINARY_FSIFOR. isf1 = interface segment save file to be created (default = infmak) isf2 = existing interface segment save file to be used (user specified) rlf = binary plot file for dynamic relaxation (default = d3drfl) efl = echo file containing optional input echo with or without node/element data root = root file name for general print option scl = scale factor for binary file sizes (default =70) cpu = cumulative cpu time limit in seconds for the entire simulation, including all restarts, if cpu is positive. If cpu is negative, the absolute value of cpu is the cpu time limit in seconds for the first run and for each subsequent restart run. kill = if LS-DYNA encounters this file name it will terminate with a restart file (default = d3kil) Getting Started vda = VDA/IGES database for geometrical surfaces c3d = CAL3D input file bof = *FREQUENCY_DOMAIN_ACOUSTIC_BEM output file nwds = Number of words to be allocated. On engineering workstations a word isusually 32bits. This number overwrites the memory size specified on the *KEYWORD card at the beginning of the input deck. dll = The dynamic library for user subroutines. Only one dynamic library can be loaded via “module=dll”. See *MODULE_LOAD command for load- ing multiple dynamic libraries. ncpu = Overrides NCPU and CONST defined in *CONTROL_PARALLEL. A positive value sets CONST = 2 and a negative values sets CONST = 1. See the *CONTROL_PARALLEL command for an explanation of these pa- rameters. The *KEYWORD command provides an alternative way to set the number of CPUs. para = Overrides PARA defined in *CONTROL_PARALLEL. time = Overrides ENDTIM defined in *CONTROL_TERMINATION. ncycle = Overrides ENDCYC defined in *CONTROL_TERMINATION. jobid = Character string which acts as a prefix for all output files. Maximum length is 72 characters. Do not include the following characters: ) (* / ? \. d3prop = See *DATABASE_BINARY_D3PROP input parameter IFILE for options. gminp = Input file for reading recorded motions in *INTERFACE_SSI (default = gmbin). gmout = Output file for writing recorded motions in *INTERFACE_SSI_AUX (default = gmbin). In order to avoid undesirable or confusing results, each LS-DYNA run should be performed in a separate directory, unless using the command line parameter “jobid” described above. If rerunning a job in the same directory, old files should first be removed or renamed to avoid confusion since the possibility exists that the binary database may contain results from both the old and new run. By including “keyword” anywhere on the execute line or instead if *KEYWORD is the first card in the input file, the keyword formats are expected; otherwise, the older structured input file will be expected. To run a coupled thermal analysis the command “couple” must be in the execute line. A thermal only analysis may be run by including the word “thermal” in the execution line. Getting Started The execution line option “pgpkey” will output the current public PGP key used by LS- DYNA for encryption of input. The public key and some instructions on how to use the key are written to the screen as well as a file named “lstc_pgpkey.asc”. The “init” (or sw1. can be used instead) command on the execution line causes the calculation to run just one cycle followed by termination with a full restart file. No editing of the input deck is required. The calculation can then be restarted with or without any additional input. Sometimes this option can be used to reduce the memory on restart if the required memory is given on the execution line and is specified too large in the beginning when the amount of required memory is unknown. Generally, this option would be used at the beginning of a new calculation. If the word “case” appears on the command line, then *CASE statements will be handled by the built in driver routines. Otherwise they should be processed by the external “lscasedriver” program, and if any *CASE statements are encountered it will cause an error. If “mcheck=y” is given on the command line, the program switches to “model check” mode. In this mode the program will run only 10 cycles – just enough to verify that the model will start. For implicit problems, all initialization is performed, but execution halts before the first cycle. If the network license is being used, the program will attempt to check out a license under the program name “LS-DYNAMC” so as not to use up one of the normal DYNA licenses. If this fails, a normal execution license will be used. If the word “memory” is found anywhere on the execution line and if it is not set via “memory=nwds” LS-DYNA will give the default size of memory, request, and then read in the desired memory size. This option is necessary if the default value is insufficient memory and termination occurs as a result. Occasionally, the default value is too large for execution and this option can be used to lower the default size. Memory can also be specified on the *KEYWORD card. SENSE SWITCH CONTROLS The status of an in-progress LS-DYNA simulation can be determined by using the sense switch. On UNIX versions, this is accomplished by first typing a “^C” (Control-C). This sends an interrupt to LS-DYNA which is trapped and the user is prompted to input the sense switch code. LS-DYNA has nine terminal sense switch controls that are tabulated below: Response A restart file is written and LS-DYNA terminates. Type SW1. Getting Started Type SW2. SW3. SW4. SW5. SW7. SW8. SW9. SWA. lprint Response LS-DYNA responds with time and cycle numbers. A restart file is written and LS-DYNA continues. A plot state is written and LS-DYNA continues. Enter interactive graphics phase and real time visualization. Turn off real time visualization. Interactive 2D rezoner visualization. for solid elements and real time Turn off real time visualization (for option SW8). Flush ASCII file buffers. Enable/Disable printing of equation solver memory, cpu requirements. nlprint Enable/Disable printing of nonlinear equilibrium information. iteration iter conv stop Enable/Disable output of binary plot database "d3iter" showing mesh after each equilibrium iteration. Useful for debugging convergence problems. Temporarily override nonlinear convergence tolerances. Halt execution immediately, closing open files. On UNIX/LINUX and Windows systems the sense switches can still be used if the job is running in the background or in batch mode. To interrupt LS-DYNA simply create a file called d3kil containing the desired sense switch, e.g., "sw1." LS-DYNA periodically looks for this file and if found, the sense switch contained therein is invoked and the d3kil file is deleted. A null d3kil file is equivalent to a "sw1." When LS-DYNA terminates, all scratch files are destroyed: the restart file, plot files, and high-speed printer files remain on disk. Of these, only the restart file is needed to continue the interrupted analysis. Getting Started PROCEDURE FOR LS-DYNA/MPP As described above the serial/SMP code supports the use of the SIGINT signal (usually Ctrl-C) to interrupt the execution and prompt the user for a "sense switch." The MPP code also supports this capability. However, on many systems a shell script or front end program (generally "mpirun") is required to start MPI applications. Pressing Ctrl-C on some systems will kill this process, and thus kill the running MPP-DYNA executable. On UNIX/LINUX systems, as workaround, when the MPP code begins execution it creates a file named, “bg_switch”, in the current working directory. This file contains the following single line: rsh <machine name> kill -INT <PID> where <machine name> is the hostname of the machine on which the root MPP-DYNA process is running, and <PID> is its process id. (on HP systems, "rsh" is replaced by "remsh"). Thus, simply executing this file will send the appropriate signal. For Windows, usually the D3KIL file is used to interrupt the execution. For more information about running the LS-DYNA/MPP Version see Appendix O. Input Stress Initialization Restart Interface Segment VDA Geometry I= = R= L= V = = Thermal File = CAL3D Input Getting Started Files: Input and Output Restart Files D=d3dump A=runrsf Z= Restart Dump Running Dump Interface Segment LS-DYNA Binary Output G=d3plot F=d3dht S= B=d3drfl "d3plot" Time History Interface Force Dynamic Relaxation O=d3hsp E= Text Output Printer File "messag" Input Echo Others... Figure 2-2. Files Input and Output. 1. Uniqueness. File names must be unique. FILES 2. Interface forces. The interface force file is created only if it is specified on the execution line “S=iff”. 3. File size limits. For very large models, the default size limits for binary output files may not be large enough for a single file to hold even a single plot state, in Getting Started which case the file size limit may be increased by specifying “X=scl" on the execution line. The default file size limit (X=70) is 70 times one-million octal words or 18.35 Mwords. That translates into 73.4 Mbytes (for 32-bit output) or 146.8 Mbytes (for 64-bit output). 4. CPU limits. Using “C=cpu” defines the maximum CPU usage allowed. When the CPU usage limit is exceeded LS-DYNA will terminate with a restart file. During a restart, cpu should be set to the total CPU used up to the current restart plus whatever amount of additional time is wanted. 5. File usage in restart. When restarting from a dump file, the execution line becomes LS-DYNA I=inf O=otf G=ptf D=dpf R=rtf F=thf T=tpf A=rrd S=iff Z=isf1 L=isf2 B=rlf W=root E=efl X=scl C=cpu K=kill Q=option KEYWORD MEMORY=nwds where, rtf=[name of dump file written by LS-DYNA] The root names of the dump files written by LS-DYNA = are controlled by dpf (default = d3dump) and rrd (default = runrsf). A two-digit number follows the root name, e.g., d3dump01, d3dump02, etc., to distinguish one dump file from another. Typically, each dump file corresponds to a different simulation time. The adaptive dump files contain all information required to successfully restart so that no other files are needed except when CAD surface data is used. When restarting a problem that uses VDA/IGES surface data, the vda input file must be specified, e.g.: LS-DYNA R=d3dump01 V=vda If the data from the last run is to be remapped onto a new mesh, then specify: “Q=remap”. The remap file is the dump file from which the remapping data is taken. The remap option is available in SMP for brick elements only, MPP does not support this option currently. No stress initialization is possible at restart. Also the VDA files and the CAL3D files must not be changed. 6. Default file names. File name dropouts are permitted; for example, the following execution lines are acceptable: LS-DYNA I=inf and Getting Started LS-DYNA R=rtf 7. Interface segments. For an analysis using interface segments, the execution line in the first analysis is given by: and in the second by: LS-DYNA I=inf Z=isf1 LS-DYNA I=inf L=isf1 8. Batch execution. In some installations (e.g., GM) calculations are controlled by a file called “names” on unit 88. The names files consists of two lines in which the second line is blank. The first line of names contains the execution line, for instance: For a restart the execution line becomes: I=inf I=inf R=rtf RESTART ANALYSIS The LS-DYNA restart capability allows analyses to be broken down into stages. After the completion of each stage in the calculation a “restart dump” is written that contains all information necessary to continue the analysis. The size of this “dump” file is roughly the same size as the memory required for the calculation. Results can be checked at each stage by post-processing the output databases in the normal way, so the chance of wasting computer time on incorrect analyses is reduced. The restart capability is frequently used to modify models by deleting excessively distorted elements, materials that are no longer important, and contact surfaces that are no longer needed. Output frequencies of the various databases can also be altered. Often, these simple modifications permit a calculation that might otherwise not to continue on to a successful completion. Restarting can also help to diagnose why a model is giving problems. By restarting from a dump that is written before the occurrence of a numerical problem and obtaining output at more frequent intervals, it is often possible to identify where the first symptoms appear and what aspect of the model is causing them. The format of the restart input file is described in this manual. If, for example, the user wishes to restart the analysis from dump state nn, contained in file D3DUMPnn, then the following procedure is followed: Getting Started 1. Create the restart input deck, if required, as described in the Restart Section of this manual. Call this file restartinput. 2. Start dyna from the command line by invoking: LS-DYNA I=restartinput R=D3DUMPnn 3. If no alterations to the model are made, then the execution line: LS-DYNA R=D3DUMPnn will suffice. Of course, the other output files should be assigned names from the command line if the defaults have been changed in the original run. The full deck restart option allows the user to begin a new analysis, with deformed shapes and stresses carried forward from a previous analysis for selected materials. The new analysis can be different from the original, e.g., more contact surfaces, different geometry (of parts which are not carried forward), etc. Examples of applications include: • Crash analysis continued with extra contact surfaces; • Sheet metalforming continued with different tools for modeling a multi-stage forming process. A typical restart file scenario: Dyna is run using an input file named “job1.inf”, and a restart dump named “d3dump01” is created. A new input file, “job2.inf”, is generated and submitted as a restart with, “R=d3dump01”, as the dump file. The input file job2.inf contains the entire model in its original undeformed state but with more contact surfaces, new output databases, and so on. Since this is a restart job, information must be given to tell LS-DYNA which parts of the model should be initialized in the full deck restart. When the calculation begins the restart database contained in the file d3dump01 is read, and a new database is created to initialize the model in the input file, job2.inf. The data in file job2.inf is read and the LS-DYNA proceeds through the entire input deck and initialization. At the end of the initialization process, all the parts selected are initialized from the data saved from d3dump01. This means that the deformed position and velocities of the nodes on the elements of each part, and the stresses and strains in the elements (and, if the material of the part is rigid, the rigid body properties) will be assigned. It is assumed during this process that any initialized part has the same elements, in the same order, with the same topology, in job1 and job2. If this is not the case, the parts cannot be initialized. However, the parts may have different identifying numbers. Getting Started For discrete elements and seat belts, the choice is all or nothing. All discrete and belt elements, retractors, sliprings, pretensioners and sensors must exist in both files and will be initialized. Materials which are not initialized will have no initial deformations or stresses. However, if initialized and non-initialized materials have nodes in common, the nodes will be moved by the initialized material causing a sudden strain in the non-initialized material. This effect can give rise to sudden spikes in loading. Points to note are: • Time and output intervals are continuous with job1, i.e., the time is not reset to zero. • Don’t try to use the restart part of the input to change anything since this will be overwritten by the new input file. • Usually, the complete input file part of job2.inf will be copied from job1.inf, with the required alterations. We again mention that there is no need to update the nodal coordinates since the deformed shapes of the initialized materials will be carried forward from job1. • Completely new databases will be generated with the time offset. VDA/IGES DATABASES VDA surfaces are surfaces of geometric entities which are given in the form of polynomials. The format of these surfaces is as defined by the German automobile and supplier industry in the VDA guidelines, [VDA 1987]. The advantage of using VDA surfaces is twofold. First, the problem of meshing the surface of the geometric entities is avoided and, second, smooth surfaces can be achieved which are very important in metalforming. With smooth surfaces, artificial friction introduced by standard faceted meshes with corners and edges can be avoided. This is a big advantage in springback calculations. A very simple and general handling of VDA surfaces is possible allowing arbitrary motion and generation of surfaces. For a detailed description, see Appendix L. Getting Started ASCII Databases Plot Files: d3plot d3thdt Geometry: i= iges: v= vda: Project: p= Keyword: k= Command: c= Database: d= LS-PrePost Nastran: n= Graphic Output Fringe Plots Time History Animations Keyword Files Project File (*.proj) Command File: cfile Database File: post.db Figure 2-3. File Organization LS-PrePost® LS-DYNA is designed to operate with a variety of commercial pre- and post-processing packages. Currently, direct support is available from TRUEGRID, PATRAN, eta/VPG, HYPERMESH, EASi-CRASH DYNA and FEMAP. Several third-party translation programs are available for PATRAN and IDEAS. Alternately, the pre- and post-processor LS-PrePost is available from LSTC and is specialized for LS-DYNA. LS-PrePost is an advanced pre- and post-processor that is delivered free with LS-DYNA. The user interface is designed to be both efficient and intuitive. LS-PrePost runs on Windows, Linux, and Unix, utilizing OpenGL graphics to achieve fast model rendering and XY plotting. Some of the capabilities available in LS-PrePost are: • Complete support for all LS-DYNA keyword data. • Importing and combining multiple models from many sources (LS-DYNA keyword, IDEAS neutral file, NASTRAN bulk data, STL ASCII, and STL binary formats). • Improved renumbering of model entities. • Model Manipulation: Translate, Rotate, Scale, Project, Offset, Reflect Getting Started • LS-DYNA Entity Creation: Coordinate Systems, Sets, Parts, Masses, CNRBs, Boxes, Spot welds, SPCs, Rigidwalls, Rivets, Initial Velocity, Accelerometers, Cross Sections, etc. • Mesh Generation: 2Dmesh Sketchboard, nLine Meshing, Line sweep into shell, Shell sweep into solid, Tet-Meshing, Automatic surface meshing of IGES and VDA data, Meshing of simple geometric objects (Plate, Sphere, Cylinder) • Special Applications: Airbag folding, Dummy positioning, Seatbelt fitting, Initial penetration check, Spot weld generation using MAT_100 • Complete support of LS-DYNA results data file: d3plot file, d3thdt file, All ASCII time history data file, Interface force file LS-PrePost processes output from LS-DYNA. LS-PrePost reads the binary plot-files generated by LS-DYNA and plots contours, fringes, time histories, and deformed shapes. Color contours and fringes of a large number of quantities may be interactively plotted on meshes consisting of plate, shell, and solid type elements. LS-PrePost can compute a variety of strain measures, reaction forces along constrained boundaries. LS-DYNA generates three binary databases. One contains information for complete states at infrequent intervals; 50 to 100 states of this sort is typical in a LS-DYNA calculation. The second contains information for a subset of nodes and elements at frequent intervals; 1000 to 10,000 states is typical. The third contains interface data for contact surfaces. Getting Started 24 20 16 12 8 4 0 20.01 8.84 1.07 1.25 1.28 1.49 2.45 2.80 BT BTW BL BWC CHL HL FBT CFHL FHL Element type Figure 2-4. Relative cost of the four noded shells available in LS-DYNA where BT is the Belytschko-Tsay shell, BTW is the Belytschko-Tsay shell with the warping stiffness taken from the Belytschko-Wong-Chiang, BWC, shell. The BL shell is the Belytschko-Leviathan shell. CHL denotes the Hughes-Liu shell, HL, with one point quadrature and a co-rotational formulation. FBT is a Belytschko-Tsay like shell with full integration, FHL is the fully integrated Hughes-Liu shell, and the CFHL shell is its co-rotational version. EXECUTION SPEEDS The relative execution speeds for various elements in LS-DYNA are tabulated below: Element Type Relative Cost 8 node solid with 1 point integration and default hourglass control as above but with Flanagan-Belytschko hourglass control constant stress and Flanagan-Belytschko hourglass control, i.e., the Flanagan-Belytschko element 4 node Belytschko-Tsay shell with four thickness integration points 4 node Belytschko-Tsay shell with resultant plasticity 4 5 7 4 Element Type Relative Cost Getting Started BCIZ triangular shell with four thickness integration points Co triangular shell with four thickness integration points 2 node Hughes-Liu beam with four integration points 2 node Belytschko-Schwer beam 2 node simple truss elements 7 4 9 2 1 8 node solid-shell with four thickness integration points 11 These relative timings are very approximate. Each interface node of the sliding interfaces is roughly equivalent to one-half zone cycle in cost. Figure 2-4. illustrates the relative cost of the various shell formulations in LS-DYNA. UNITS The units in LS-DYNA must be consistent. One way of testing whether a set of units is consistent is to check that: [force unit] = [mass unit] × [acceleration unit] and that [acceleration unit] = [length unit] [time unit]2 . Examples of sets of consistent units are tabulated below. For a more comprehensive table, see http://ftp.lstc.com/anonymous/outgoing/support/FAQ/consistent_units . (a) (b) (c) Length unit Time unit Mass unit Force unit Young’s Modulus of Steel Density of Steel Yield stress of Mild Steel Acceleration due to gravity Velocity equivalent to 30 mph meter second kilogram Newton 210.0E+09 7.85E+03 200.0E+06 9.81 13.4 millimeter second tonne Newton 210.0E+03 7.85E–09 200.0 9.81E+03 13.4E+03 millimeter millisecond kilogram kiloNewton 210.0 7.85E–06 0.200 9.81E-03 13.4 Getting Started GENERAL CARD FORMAT The following sections specify, for each keyword command, the cards that must be defined and those cards that are optional. Each card is described in its fixed format form and is shown as a number of fields in an 80 character string. With the exception of “long format input” as described later in this section, most cards are 8 fields with a field length of 10 characters. A sample card is shown below. The card format is clearly stated when it is different than 8 fields of 10 characters. As an alternative to fixed format, a card may be in free format with the values of the variables separated by commas. When using comma-delimited values on a card, the number of characters used to specify a value must not exceed the field length for fixed format. For example, an I8 number is limited to a value of 99999999 and a larger number with more than 8 characters is unacceptable. A further restriction is that characters beyond column 80 of each line are ignored by the code. Fixed format and free, comma-delimited format can be mixed throughout the deck and even within different cards of a single command but not within a card. The limits on number of characters per variable and number of characters per line as stated above are raised in the case of long format input. See the description of long format input below. Example Card. Card [N] 1 2 Variable NSID PSID Type I I 3 A1 F 4 A2 F Default none none 1.0 1.0 Remarks 1 2 5 A3 F 0 6 KAT I 1 3 7 8 In the example shown above, the row labeled “Type” gives the variable type and is either F, for floating point or I, for an integer. The row labeled “Default” reveals the default value set for a variable if zero is specified, the field is left blank, or the card is not defined. The “Remarks” row refers to enumerated remarks at the end of the section. Getting Started Optional Cards: Each keyword card (line beginning with “*”) is followed by a set of data cards. Data cards are either, 1. Required Cards. Unless otherwise indicated, cards are required. 2. Conditional Cards. Conditional cards are required provided some condition is satisfied. The following is a typical conditional card: ID Card. Additional card for the ID keyword option. ID 1 2 3 4 5 6 7 8 Variable ABID Type I HEADING A70 3. Optional Cards. An optional card is one that may be replaced by the next keyword card. The fields in the omitted optional data cards are assigned their default values. Example. Suppose the data set for *KEYWORD consists of 2 required cards and 3 optional cards. Then, the fourth card may be replaced by the next key- word card. All the fields in the omitted fourth and fifth cards are assigned their default values. WARNING: In this example, even though the fourth card is optional, the input deck may not jump from the third to fifth card. The only card that card 4 may be replaced with is the next keyword card. Long Format Input: To accommodate larger or more precise values for input variables than are allowed by the standard format input as described above, a “long format” input option is available. One way of invoking long format keyword input is by adding “long=y” to the execution line. A second way is to add “long=y” to the *KEYWORD command in the input deck. long=y: read long keyword input deck; write long structured input deck. long=s: read standard keyword input deck; write long structured input deck. long=k: read long keyword input deck; write standard structured input deck. Getting Started The “long=s” option may be helpful in the rare event that the keyword input is of standard format but LS-DYNA reports an input error and the dyna.str file reveals that one of more variables is incorrectly written to dyna.str as a series of asterisks due to inadequate field length(s) in dyna.str. The “long=k” option really serves no practical purpose. When long format is invoked for keyword input, field lengths for each variable become 20 characters long (160 character limit per line for 8 variables; 200 character limit per line for 10 variables). In this way, the number of input lines in long format is unchanged from regular format. To convert a standard format input deck to a long format input deck, run LS-DYNA with “newformat = long” on the execution line. For example, if standard.k is a standard format input deck, ls-dyna i = standard.k newformat = long will create a long format input deck called standard.k.long. You can mix long and standard format within one input deck by use of “+” or “-“ signs within the deck. If the execution line indicates standard format, you can add “ +” at the end of any keywords to invoke long format just for those keywords. For example, “*NODE +” in place of “*NODE” invokes a read format of two lines per node (I20, 3E20.0 on the first line and 2F20.0 on the second line). Similarly, if the execution line indicates long format, you can add “-” at the end of any keywords to invoke standard format for those keywords. For example, “*NODE –” in place of “*NODE” invokes the standard read format of one line per node (I8, 3E16.0, 2F8.0). Taking this idea a step further, adding a “-” or “+” to the end of the *INCLUDE keyword command signals to LS-DYNA that all the commands in the included file are standard format or long format, respectively. Purpose: Define an airbag or control volume. The keyword *AIRBAG provides a way of defining thermodynamic behavior of the gas flow into the airbag as well as a reference configuration for the fully inflated bag. The keyword cards in this section are defined in alphabetical order: *AIRBAG_OPTION1_{OPTION2}_{OPTION3}_{OPTION4} *AIRBAG_ADVANCED_ALE *AIRBAG_ALE *AIRBAG_INTERACTION *AIRBAG_PARTICLE *AIRBAG_REFERENCE_GEOMETRY_OPTION_OPTION *AIRBAG_SHELL_REFERENCE_GEOMETRY *AIRBAG_OPTION1_{OPTION2}_{OPTION3}_{OPTION4} OPTION1 specifies one of the following thermodynamic models: SIMPLE_PRESSURE_VOLUME SIMPLE_AIRBAG_MODEL ADIABATIC_GAS_MODEL WANG_NEFSKE WANG_NEFSKE_JETTING WANG_NEFSKE_MULTIPLE_JETTING LOAD_CURVE LINEAR_FLUID HYBRID HYBRID_JETTING HYBRID_CHEMKIN FLUID_AND_GAS OPTION2 specifies that an additional line of data is read for the WANG_NEFSKE type thermodynamic relationships. The additional data controls the initiation of exit flow from the airbag. OPTION2 takes the single option: POP OPTION3 specifies that a constant momentum formulation is used to calculate the jetting load on the airbag an additional line of data is read in: OPTION3 takes the single option: CM OPTION4 given by: ID Specifies that an airbag ID and heading information will be the first card of the airbag definition. This ID is a unique number that is necessary for the identification of the airbags in the definition of airbag interaction via *AIRBAG_INTERACTION keyword. The numeric ID's and heading are written into the abstat and d3hsp files. Core Cards: Common to all airbags ID Card. Additional card for the ID keyword option. To use the *AIRBAG_INTERAC- TION keyword ID Cards are required. ID 1 2 3 4 5 6 7 8 Variable ABID Type I HEADING A70 Card 1a 1 2 3 4 5 6 7 8 Variable SID SIDTYP RBID VSCA PSCA VINI MWD SPSF Type I Default none I 0 I 0 F 1. F 1. F 0. F 0. F 0. Remark optional VARIABLE DESCRIPTION ABID Airbag ID. This must be a unique number. HEADING Airbag descriptor. It is suggested that unique descriptions be used. SID Set ID SIDTYP Set type: EQ.0: segment, NE.0: part set ID. DESCRIPTION *AIRBAG RBID Rigid body part ID for user defined activation subroutine: LT.0: -RBID is taken as the rigid body part ID. Built in sensor subroutine initiates the inflator. Load curves are offset by initiation time. EQ.0: The control volume is active from time zero. GT.0: RBID is taken as the rigid body part ID. User sensor subroutine initiates the inflator. Load curves are offset by initiation time. See Appendix D. Volume scale factor (default = 1.0) Pressure scale factor (default = 1.0) Initial filled volume Mass weighted damping factor, D Stagnation pressure scale factor, 0 <= 𝛾 <= 1 VSCA PSCA VINI MWD SPSF Remarks: The first card is necessary for all airbag options. The option dependent cards follow. Lumped parameter control volumes are a mechanism for determining volumes of closed surfaces and applying a pressure based on some thermodynamic relation. The volume is specified by a list of polygons similar to the pressure boundary condition cards or by specifying a material subset which represents shell elements which form the closed boundary. All polygon normal vectors must be oriented to face outwards from the control volume, however for *AIRBAG_PARTICLE, which does not rely on control volumes, all polygon normal vectors must be oriented to face inwards to get proper volume . If holes are detected, they are assumed to be covered by planar surfaces. There are two sets of volume and pressure variables used for each control volume model. First, the finite element model computes a volume 𝑉femodel and applies a pressure 𝑃femodel. The thermodynamics of a control volume may be computed in a different unit system with its own set of varriables: 𝑉cvolume and pressure 𝑃cvolume which are used for integrating the differential equations for the control volume. The conversion is as follows: 𝑉cvolume = (VSCA × 𝑉femodel) − VINI 𝑃femodel = PSCA×𝑃cvolume Where VSCA, PSCA, and VINI are input parameters. Damping can be applied to the structure enclosing a control volume by using a mass weighted damping formula: 𝑑 = 𝑚𝑖𝐷(𝑣𝑖 − 𝑣cg) 𝐹𝑖 𝑑 is the damping force, mi is the nodal mass, 𝜈𝑖 is the velocity for a node, 𝑣cg is where 𝐹𝑖 the mass weighted average velocity of the structure enclosing the control volume, and D is the damping factor. An alternative, separate damping is based on the stagnation pressure. The stagnation pressure is roughly the maximum pressure on a flat plate oriented normal to a steady state flow field. The stagnation pressure is defined as 𝑝 = 𝛾𝜌𝑉2 where 𝑉 is the normal velocity of the control volume relative to the ambient velocity, 𝜌 is the ambient air density, and 𝛾 is a factor which varies from 0 to 1 and has to be chosen by the user. Small values are recommended to avoid excessive damping. Sensor input: The sensor is mounted on a rigid body which is attached to the structure. The motion of the sensor is evaluated in the local coordinate system of the rigid body. See *MAT_RIGID. This local system rotates and translates with the rigid material. The default local system for a rigid body is taken as the principal axes of the inertia tensor. When the user defined criterion for airbag deployment is satisfied, a flag is set and deployment begins. All load curves relating to the mass flow rate versus time are then shifted by the initiation time. RBID = 0: No rigid body For this case there is no rigid body, and the control volume is active from time zero. There are no additional sensor cards. RBID > 0: User supplied sensor subroutine The value of RBID is taken as a rigid body part ID, and a user supplied sensor subroutine will be called to determine the flag that initiates deployment. See Appendix D for details regarding the user supplied subroutine. For RBID > 0 the additional cards are specified below: User Subroutine Control Card. This card is read in when RBID > 0. 2 3 4 5 6 7 8 Card 1b Variable Type 1 N I Default none User Subroutine Constant Cards. Define N constants for the user subroutine. Include only the number of cards necessary, i.e. for nine constants use 2 cards. Card 1c Variable 1 C1 Type F Default 0. 2 C2 F 0. 3 C3 F 0. 4 C4 F 0. 5 C5 F 0. 6 7 8 VARIABLE DESCRIPTION N Number of input parameters (not to exceed 25). C1, …, CN Up to 25 constants for the user subroutine. RBID < 0: User supplied sensor subroutine The value of –RBID is taken as rigid body part ID and a built in sensor subroutine is called. For RBID < 0 there are three additional cards. Acceleration Sensor Card. Card 1d Variable 1 AX Type F Default 0. 2 AY F 0. 3 AZ F 0. Velocity Sensor Card. 4 5 6 7 8 AMAG TDUR F 0. F 0. Card 1e 1 2 3 4 5 6 7 8 Variable DVX DVY DVZ DVMAG Type F Default 0. F 0. Displacement Sensor Card. Card 1f Variable 1 UX Type F Default 0. 2 UY F 0. F 0. 3 UZ F 0. F 0. 4 5 6 7 8 UMAG F 0. AX AY AZ *AIRBAG DESCRIPTION Acceleration level in local 𝑥-direction to activate inflator. The absolute value of the 𝑥-acceleration is used. EQ.0: inactive. Acceleration level in local 𝑦-direction to activate inflator. The absolute value of the 𝑦-acceleration is used. EQ.0: inactive. Acceleration level in local 𝑧-direction to activate inflator. The absolute value of the 𝑧-acceleration is used. EQ.0: inactive. AMAG Acceleration magnitude required to activate inflator. EQ.0: inactive. TDUR DVX DVY DVZ Time duration acceleration must be exceeded before the inflator activates. This is the cumulative time from the beginning of the calculation, i.e., it is not continuous. Velocity change in local 𝑥-direction to activate the inflator. (The absolute value of the velocity change is used.) EQ.0: inactive. Velocity change in local 𝑦-direction to activate the inflator. (The absolute value of the velocity change is used.) EQ.0: inactive. Velocity change in local 𝑧-direction to activate the inflator. (The absolute value of the velocity change is used.) EQ.0: inactive. DVMAG Velocity change magnitude required to activate the inflator. EQ.0: inactive. UX Displacement increment in local 𝑥-direction to activate the inflator. (The absolute value of the 𝑥-displacement is used.) EQ.0: inactive. UY UZ *AIRBAG DESCRIPTION Displacement increment in local 𝑦-direction to activate the inflator. (The absolute value of the 𝑦-displacement is used.) EQ.0: inactive. Displacement increment in local 𝑧-direction to activate the inflator. (The absolute value of the 𝑧-displacement is used.) EQ.0: inactive. UMAG Displacement magnitude required to activate the inflator. EQ.0: inactive. *AIRBAG_SIMPLE_PRESSURE_VOLUME_OPTION Additional card for SIMPLE_PRESSURE_VOLUME option. (For card 1 see the “core cards” section of *AIRBAG.) Card 2 Variable 1 CN 2 3 4 5 6 7 8 BETA LCID LCIDDR Type F F I Default none none none I 0 VARIABLE DESCRIPTION CN Coefficient. Define if the load curve ID, LCID, is unspecified. LT.0.0: |CN| is the load curve ID, which defines the coefficient as a function of time. Scale factor, 𝛽. Define if a load curve ID is not specified. Optional load curve ID defining pressure versus relative volume. Optional load curve ID defining the coefficient, CN, as a function of time during the dynamic relaxation phase. BETA LCID LCIDDR Remarks: The relationship is the following: Pressure = 𝛽 × CN Relative Volume Relative Volume = Current Volume Initial Volume The pressure is then a function of the ratio of current volume to the initial volume. The constant, CN, is used to establish a relationship known from the literature. The scale factor 𝛽 is simply used to scale the given values. This simple model can be used when an initial pressure is given and no leakage, no temperature, and no input mass flow is assumed. A typical application is the modeling of air in automobile tires. The load curve, LCIDDR, can be used to ramp up the pressure during the dynamic relaxation phase in order to avoid oscillations after the desired gas pressure is reached. In the DEFINE_CURVE section this load curve must be flagged for dynamic relaxation. After initialization either the constant or load curve ID, |CN| is used to determine the pressure. *AIRBAG_SIMPLE_AIRBAG_MODEL_OPTION Additional cards for SIMPLE_AIRBAG_MODEL option. (For card 1 see the “core cards” section of *AIRBAG.) Card 2 Variable 1 CV Type F 2 CP F 3 T F 4 5 6 LCID MU AREA I F F 7 PE F 8 RO F Default none none none none none none none none Card 3 1 2 Variable LOU T_EXT Type Default Remarks I 0 0 F 0. 3 A F 4 B F 0. 0. 5 6 7 8 MW GASC F 0. F 0. optional optional optional optional optional VARIABLE DESCRIPTION CV CP T LCID Heat capacity at constant volume, e.g., Joules/kg/oK. Heat capacity at constant pressure, e.g., Joules/kg/oK. Temperature of input gas Load curve ID specifying input mass flow rate. See *DEFINE_- CURVE. MU Shape factor for exit hole, 𝜇: LT.0.0: ∣𝜇∣ is the load curve number defining the shape factor as a function of absolute pressure. VARIABLE DESCRIPTION AREA Exit area, A: GE.0.0: A is the exit area and is constant in time, LT.0.0: |A| is the load curve number defining the exit area as a function of absolute pressure. PE RO LOU Ambient pressure, 𝑝𝑒 Ambient density, 𝜌 Optional load curve ID giving mass flow out versus gauge pressure in bag. See *DEFINE_CURVE. Leave the following 5 fields blank blank if CV ≠ 0 T_EXT Ambient temperature. First heat Joules/mole/oK). capacity Second heat Joules/mole/oK2). capacity coefficient of inflator gas (e.g., coefficient of inflator gas, (e.g., Molecular weight of inflator gas (e.g., Kg/mole). Universal Joules/mole/oK). gas constant of inflator gas (e.g., 8.314 A B MW GASC Remarks: The gamma law equation of state used to determine the pressure in the airbag: 𝑝 = (𝛾 − 1)𝜌𝑒 where p is the pressure, 𝜌 is the density, 𝑒 is the specific internal energy of the gas, and 𝛾 is the ratio of the specific heats: 𝛾 = 𝑐𝑝 𝑐𝑣 From conservation of mass, the time rate of change of mass flowing into the bag is given as: 𝑑𝑀 𝑑𝑡 = 𝑑𝑀in 𝑑𝑡 − 𝑑𝑀out 𝑑𝑡 The inflow mass flow rate is given by the load curve ID, LCID. Leakage, the mass flow rate out of the bag, can be modeled in two alternative ways. One is to give an exit area with the corresponding shape factor, then the load curve ID, LOU, must be set to zero. The other is to define a mass flow out by a load curve, then 𝜇 and A have to both be set to zero. If CV = 0. then the constant-pressure specific heat is given by: and the constant-volume specific heat is then found from: 𝑐𝑝 = (𝑎 + 𝑏𝑇) MW 𝑐𝑣 = 𝑐𝑝 − MW *AIRBAG_ADIABATIC_GAS_MODEL_OPTION Additional card for ADIABATIC_GAS_MODEL option. (For card 1 see the “core cards” section of *AIRBAG.) Card 2 1 2 3 Variable PSF LCID GAMMA Type F I F 4 P0 F 5 PE F 6 RO F 7 8 Default 1.0 none none none none none VARIABLE DESCRIPTION PSF LCID Pressure scale factor Optional load curve for preload flag. See *DEFINE_CURVE. GAMMA Ratio of specific heats P0 PE RO Initial pressure (gauge) Ambient pressure Initial density of gas Remarks: The optional load curve ID, LCID, defines a preload flag. During the preload phase the function value of the load curve versus time is zero, and the pressure in the control volume is given as: 𝑝 = PSF × 𝑝0 When the first nonzero function value is encountered, the preload phase stops and the ideal gas law applies for the rest of the analysis. If LCID is zero, no preload is performed. The gamma law equation of state for the adiabatic expansion of an ideal gas is used to determine the pressure after preload: 𝑝 = (𝛾 − 1)𝜌𝑒 where p is the pressure, 𝜌 is the density, e is the specific internal energy of the gas, and 𝛾 is the ratio of the specific heats: 𝛾 = 𝑐𝑝 𝑐𝑣 The pressure above is the absolute pressure, the resultant pressure acting on the control volume is: 𝑝𝑠 = PSF × (𝑝 − 𝑝𝑒) where PSF is the pressure scale factor. Starting from the initial pressure 𝑝0 an initial internal energy is calculated: 𝑒0 = 𝑝0 + 𝑝𝑒 𝜌(𝛾 − 1) *AIRBAG The following sequence of cards is read in for the all variations of the WANG_NEFSKE option to *AIRBAG. For card 1 see the “core cards” section of *AIRBAG. Card 2 Variable 1 CV Type F 2 CP F 3 T F Default none none 0. Card 3 1 2 3 4 5 6 7 8 LCT LCMT TVOL LCDT IABT I 0 4 I F I F none 0. 0. not used 5 6 7 8 Variable C23 LCC23 A23 LCA23 CP23 LCCP23 AP23 LCAP23 Type F Default none Card 4 Variable 1 PE Type F I 0 2 RO F F none 3 GC F Default none none none I 0 4 F none 5 I 0 6 F 0.0 7 I 0 8 LCEFR POVER PPOP OPT KNKDN I 0 F F F 0.0 0.0 0.0 I Inflator Card. If the inflator is modeled, LCMT = 0 fill in the following card. If not, include but leave blank. Card 5 1 2 3 4 Variable IOC IOA IVOL IRO Type F F F F 5 IT F 6 7 8 LCBF I Default none none none none none none Temperature Dependent Heat Capacities Card. Include this card when CV = 0. Card 6 1 Variable TEXT Type F 2 A F 3 B F 4 5 6 7 8 MW GASC HCONV F F F Default none none none none none none Criteria for Initiating Exit Flow Card. Additional card for the POP option to the *AIRBAG_WANG_NEFSKE card. Card 7 1 2 3 4 5 6 7 8 Variable TDP AXP AYP AZP AMAGP TDURP TDA RBIDP Type F F F F F F F I Default 0.0 0.0 0.0 0.0 0.0 0.0 0.0 none VARIABLE DESCRIPTION CV CP T Specific heat at constant volume, e.g., Joules/kg/oK. Specific heat at constant pressure, e.g., Joules/kg/oK. Temperature of input gas. For temperature variations a load curve, LCT, may be defined. VARIABLE DESCRIPTION LCT LCMT TVOL LCDT IABT C23 LCC23 A23 LCA23 Optional load curve number defining temperature of input gas versus time. This overrides columns T. Load curve specifying input mass flow rate or tank pressure versus time. If the tank volume, TVOL, is nonzero the curve ID is assumed to be tank pressure versus time. If LCMT = 0, then the inflator has to be modeled, see Card 5. During the dynamic relaxation phase the airbag is ignored unless the curve is flagged to act during dynamic relaxation. Tank volume which is required only for the tank pressure versus time curve, LCMT. Load curve for time rate of change of temperature (dT/dt) versus time. Initial airbag temperature. (Optional, generally not defined.) Vent orifice coefficient which applies to exit hole. Set to zero if LCC23 is defined below. The absolute value, |LCC23|, is a load curve ID. If the ID is positive, the load curve defines the vent orifice coefficient which applies to exit hole as a function of time. If the ID is negative, the vent orifice coefficient is defined as a function of relative pressure, 𝑃air/𝑃bag, see [Anagonye and Wang 1999]. In addition, LCC23 can be defined through *DEFINE_CURVE_FUNCTION. A nonzero value for C23 overrides LCC23. If defined as a positive number, A23 is the vent orifice area which applies to exit hole. If defined as a negative number, the absolute value |A23| is a part ID, see [Anagonye and Wang, 1999]. The area of this part becomes the vent orifice area. Airbag pressure will not be applied to part |A23| representing venting holes if part |A23| is not included in SID, the part set representing the airbag. Set A23 to zero if LCA23 is defined below. Load curve number defining the vent orifice area which applies to exit hole as a function of absolute pressure, or LCA23 can be defined through *DEFINE_CURVE_FUNCTION. A nonzero value for A23 overrides LCA23. CP23 Orifice coefficient for leakage (fabric porosity). Set to zero if LCCP23 is defined below. LCCP23 *AIRBAG_WANG_NEFSKE DESCRIPTION Load curve number defining the orifice coefficient for leakage (fabric porosity) as a function of time, or LCCP23 can be defined through *DEFINE_CURVE_FUNCTION. A nonzero value for CP23 overrides LCCP23. AP23 Area for leakage (fabric porosity) LCAP23 PE RO GC Load curve number defining the area for leakage (fabric porosity) as a function of (absolute) pressure, or LCAP23 can be defined through *DEFINE_CURVE_FUNCTION. A nonzero value for AP23 overrides LCAP23. Ambient pressure Ambient density Gravitational conversion constant (mandatory - no default). If consistent units are being used for all parameters in the airbag definition then unity should be input. LCEFR Optional curve for exit flow rate (mass/time) versus (gauge) pressure POVER Initial relative overpressure (gauge), Pover in control volume PPOP OPT Pop Pressure: relative pressure (gauge) for initiating exit flow, Ppop Fabric venting option, if nonzero CP23, LCCP23, AP23, and LCAP23 are set to zero. EQ.1: Wang-Nefske formulas for venting through an orifice are used. Blockage is not considered. EQ.2: Wang-Nefske formulas for venting through an orifice are used. Blockage of venting area due to contact is consid- ered. EQ.3: Leakage formulas of Graefe, Krummheuer, and Siejak [1990] are used. Blockage is not considered. EQ.4: Leakage formulas of Graefe, Krummheuer, and Siejak [1990] are used. Blockage of venting area due to contact is considered. EQ.5: Leakage formulas based on flow through a porous media are used. Blockage is not considered. VARIABLE DESCRIPTION EQ.6: Leakage formulas based on flow through a porous media are used. Blockage of venting area due to contact is con- sidered. EQ.7: Leakage is based on gas volume outflow versus pressure load curve. Blockage of flow area due to contact is not considered. Absolute pressure is used in the porous- velocity-versus-pressure load curve, given as FAC(P) in the *MAT_FABRIC card. EQ.8: Leakage is based on gas volume outflow versus pressure load curve. Blockage of flow area due to contact is con- sidered. Absolute pressure is used in the porous- velocity-versus-pressure load curve, given as FAC(P) in the *MAT_FABRIC card. Optional load curve ID defining the knock down pressure scale factor versus time. This option only applies to jetting. The scale factor defined by this load curve scales the pressure applied to airbag segments which do not have a clear line-of-sight to the jet. Typically, at very early times this scale factor will be less than unity and equal to unity at later times. The full pressure is always applied to segments which can see the jets. KNKDN IOC IOA Inflator orifice coefficient Inflator orifice area IVOL Inflator volume IRO IT LCBF TEXT A B Inflator density Inflator temperature Load curve defining burn fraction versus time Ambient temperature. First molar heat capacity coefficient of Joules/mole/oK) inflator gas (e.g., Second molar heat capacity coefficient of inflator gas, (e.g., Joules/mole/oK2) MW GASC HCONV *AIRBAG_WANG_NEFSKE DESCRIPTION Molecular weight of inflator gas (e.g., Kg/mole). Universal gas constant of inflator gas (e.g., 8.314 Joules/mole/oK) Effective heat transfer coefficient between the gas in the air bag and the environment at temperature TEXT. If HCONV < 0, then HCONV defines a load curve of data pairs (time, hconv). TDP Time delay before initiating exit flow after pop pressure is reached. AXP Pop acceleration magnitude in local x-direction. EQ.0.0: Inactive. AYP Pop acceleration magnitude in local y-direction. EQ.0.0: Inactive. AZP Pop acceleration magnitude in local z-direction. EQ.0.0: Inactive. AMAGP Pop acceleration magnitude. EQ.0.0: Inactive. Time duration pop acceleration must be exceeded to initiate exit flow. This is a cumulative time from the beginning of the calculation, i.e., it is not continuous. Time delay before initiating exit flow after pop acceleration is exceeded for the prescribed time duration. Part ID of the rigid body for checking accelerations against pop accelerations. TDURP TDA RBIDP Remarks: The gamma law equation of state for the adiabatic expansion of an ideal gas is used to determine the pressure after preload: 𝑝 = (𝛾 − 1)𝜌𝑒 where p is the pressure, 𝜌 is the density, e is the specific internal energy of the gas, and 𝛾 is the ratio of the specific heats: 𝛾 = 𝑐𝑝 𝑐𝑣 where cv is the specific heat at constant volume, and cp is the specific heat at constant pressure. A pressure relation is defined: 𝑄 = 𝑝𝑒 where pe is the external pressure and p is the internal pressure in the bag. A critical pressure relationship is defined as: 𝑄crit = ( 𝛾 + 1 𝛾−1 ) where 𝛾 is the ratio of specific heats: and 𝛾 = 𝑐𝑝 𝑐𝑣 𝑄 ≤ 𝑄crit⇒𝑄 = 𝑄crit. Wang and Nefske define the mass flow through the vents and leakage by and 𝑚̇ 23 = 𝐶23𝐴23 𝑅√𝑇2 𝛾√2𝑔𝑐 ( 𝛾𝑅 𝛾 − 1 ) (1 − 𝑄 𝛾−1 𝛾 ) 𝑚′̇ 23 = 𝐶′23𝐴′23 𝑅√𝑇2 𝛾√2𝑔𝑐 ( 𝛾𝑅 𝛾 − 1 ) (1 − 𝑄 𝛾−1 𝛾 ) It must be noted that the gravitational conversion constant has to be given in consistent units. As an alternative to computing the mass flow out of the bag by the Wang-Nefske model, a curve for the exit flow rate depending on the internal pressure can be taken. Then, no definitions for C23, LCC23, A23, LCA23, CP23, LCCP23, AP23, and LCAP23 are necessary. The airbag inflator assumes that the control volume of the inflator is constant and that the amount of propellant reacted can be defined by the user as a tabulated curve of fraction reacted versus time. A pressure relation is defined: 𝑄crit = 𝑝𝑐 𝑝𝑖 = ( 𝛾 + 1 𝛾−1 ) where 𝑝𝑐 is a critical pressure at which sonic flow occurs, 𝑝𝐼, is the inflator pressure. The exhaust pressure is given by 𝑝𝑒 = { 𝑝𝑎 𝑝𝑐 if 𝑝𝑎 ≥ 𝑝𝑐 if 𝑝𝑎 < 𝑝𝑐 where 𝑝𝑎 is the pressure in the control volume. The mass flow into the control volume is governed by the equation: √ √ √ √ 𝑔𝑐𝛾 (𝑄 𝛾 − 𝑄 𝛾+1 𝛾 ) 𝑚̇ in = 𝐶0𝐴0√2𝑝𝐼𝜌𝐼 ⎷ where 𝐶0, 𝐴0, and 𝜌𝐼 are the inflator orifice coefficient, area, and gas density, respectively. 𝛾 − 1 If OPT is defined, then for OPT set to 1 or 2 the mass flow rate out of the bag, 𝑚̇ 𝑜𝑢𝑡 is given by: nairmats 𝑚̇ 𝑜𝑢𝑡 = √𝑔𝑐 { ∑ [FLC(𝑡)𝑛 × FAC(𝑝)𝑛 × Area𝑛] } √2𝑝𝜌 𝑛=1 √ √ √ √ ⎷ 𝑘 − 𝑄 𝛾+1 𝛾 ) 𝛾 (𝑄 𝛾 − 1 where, 𝜌 is the density of airbag gas, “nairmats” is the number of fabrics used in the airbag, and “Arean” is the current unblocked area of fabric number n. If OPT set to 3 or 4 then: nairmats 𝑚̇ out = { ∑ [FLC(𝑡)𝑛 × FAC(𝑝)𝑛 × Area𝑛] } √2(𝑝 − 𝑝ext)𝜌 and for OPT set to 5 or 6: 𝑛=1 nairmats 𝑚̇ out = { ∑ [FLC(𝑡)𝑛 × FAC(𝑝)𝑛 × Area𝑛] } (𝑝 − 𝑝ext) 𝑛=1 and for OPT set to 7 or 8 (may be comparable to an equivalent model ALE model): nairmats 𝑚̇ out = ∑ FLC(𝑡)𝑛×FAC(𝑝)𝑛 × Area𝑛 × 𝜌𝑛 𝑛=1 Note that for different OPT settings, FAC(𝑝)𝑛 has different meanings (all units shown just as demonstrations): 1. For OPT of 1, 2, 3 and 4, FAC(P) is unit-less. 2. For OPT of 5 and 6, FAC(P) has a unit of (s/m). 3. For OPT of 7 or 8, FAC(P) is the gas volume outflow through a unit area per unit time thus has the unit of speed, 4. [FAC(𝑃)] = [volume] [area][𝑡] = [L]3 [L]2[𝑡] = [𝐿] [𝑡] = [velocity]. Multiple airbags may share the same part ID since the area summation is over the airbag segments whose corresponding part ID’s are known. Currently, we assume that no more than ten materials are used per bag for purposes of the output. This constraint can be eliminated if necessary. The total mass flow out will include the portion due to venting, i.e., constants C23 and A23 or their load curves above. If CV = 0. then the constant-pressure specific heat is given by: and the constant-volume specific heat is then found from: 𝑐𝑝 = (𝑎 + 𝑏𝑇) 𝑀𝑊 𝑐𝑣 = 𝑐𝑝 − 𝑀𝑊 Two additional cards are required for JETTING models: The following additional cards are defined for the WANG_NEFSKE_JETTING and WANG_NEFSKE_MULTIPLE_JETTING options, two further cards are defined for each option. The jet may be defined by specifying either the coordinates of the jet focal point, jet vector head and secondary jet focal point, or by specifying three nodes located at these positions. The nodal point option is recommended when the location of the airbag changes as a function of time. NOTE: For Jetting models define either of the two cards be- low but not both. Card format 8 for WANG_NEFSKE keyword option. Card 8 1 2 3 4 5 6 Variable XJFP YJFP ZJFP XJVH YJVH ZJVH Type F F F F F F 7 CA F 8 BETA F Default none none none none none none none 1.0 Remark 1 1 1 1 1 Card format 8 for WANG_NEFSKE_MUTTIPLE_JETTING keyword options. Card 8 1 2 3 4 5 6 7 8 Variable XJFP YJFP ZJFP XJVH YJVH ZJVH LCJRV BETA Type F F F F F F F F Default none none none none none none none 1.0 Remark 1 1 1 1 1 1 Card 9 for both WANG_NEFSKE_JETTING and WANG_NEFSKE_MULTIPLE_JET- TING. Card 9 1 2 3 4 5 6 7 8 Variable XSJFP YSJFP ZSJFP PSID ANGLE NODE1 NODE2 NODE3 Type F F F I F Default none none none none none Remark I 0 1 I 0 1 I 0 Airbag Gaussian velocity profile Virtual origin Node 1 Node 2 Hole diameter Pressure is applied to surfaces that are in the line of sight of the virtual origin. α: smaller α: larger Figure 3-1. Jetting configuration for driver's side airbag (pressure applied only if centroid of surface is in line-of-sight) Secondary focal jet point Virtual origin Node 1 Node 3 Gaussian profile Node 2 Figure 3-2. Jetting configuration for the passenger’s side bag. VARIABLE DESCRIPTION XJFP YJFP x-coordinate of jet focal point, i.e., the virtual origin in Figures 3-1 and 3-2. See Remark 1 below. y-coordinate of jet focal point, i.e., the virtual origin in Figures 3-1 and 3-2. Relative jet velocity (degrees) cut off angle, ψ for ψ > ψ cut v=0 cut Figure 3-3. Normalized jet velocity versus angle for multiple jet driver's side airbag VARIABLE DESCRIPTION ZJFP XJVH YJVH ZJVH CA LCJRV z-coordinate of jet focal point, i.e., the virtual origin in Figures 3-1 and 3-2. x-coordinate of jet vector head to defined code centerline y-coordinate of jet vector head to defined code centerline z-coordinate of jet vector head to defined code centerline Cone angle, 𝛼, defined in radians. LT.0.0: |𝛼| is the load curve ID defining cone angle as a function of time Load curve ID giving the spatial jet relative velocity distribution, see Figures 3-1, 3-2, and 3-3. The jet velocity is determined from the inflow mass rate and scaled by the load curve function value corresponding to the value of the angle 𝜓. Typically, the values on the load curve vary between 0 and unity. See *DEFINE_- CURVE. BETA Efficiency factor, 𝛽, which scales the final value of pressure obtained from Bernoulli’s equation. LT.0.0: ∣𝛽∣ is the load curve ID defining the efficiency factor as a function of time cut Figure 3-4. Multiple jet model for driver's side airbag. Typically, 𝜓cut is close to 90°. The angle 𝜓0 is included to indicate that there is some angle below which the jet is negligible; see Figure 3-3. VARIABLE XSJFP YSJFP ZSJFP PSID ANGLE DESCRIPTION x-coordinate of secondary jet focal point, passenger side bag. If the coordinates of the secondary point are (0,0,0) then a conical jet (driver’s side airbag) is assumed. y-coordinate of secondary jet focal point z-coordinate of secondary jet focal point Optional part set ID, see *SET_PART. If zero all elements are included in the airbag. Cutoff angle in degrees. The relative jet velocity is set to zero for angles greater than the cutoff. See Figure 3-3. This option applies to the MULTIPLE jet only. NODE1 Node ID located at the jet focal point, i.e., the virtual origin in Figures 3-1 and 3-2. See Remark 1 below. NODE2 Node ID for node along the axis of the jet. NODE3 Optional node ID located at secondary jet focal point. *AIRBAG_WANG_NEFSKE 1. It is assumed that the jet direction is defined by the coordinate method (XJFP, YJFP, ZJFP) and (XJVH, YJVH, ZJVH) unless both NODE1 and NODE2 are defined. In which case the coordinates of the nodes give by NODE1, NODE2 and NODE3 will override (XJFP, YJFP, ZJFP) and (XJVH, YJVH, ZJVH). The use of nodes is recommended if the airbag system is undergoing rigid body motion. The nodes should be attached to the vehicle to allow for the coordi- nates of the jet to be continuously updated with the motion of the vehicle. 2. The jetting option provides a simple model to simulate the real pressure distribution in the airbag during the breakout and early unfolding phase. Only the surfaces that are in the line of sight to the virtual origin have an increased pressure applied. With the optional load curve LCRJV, the pressure distribu- tion with the code can be scaled according to the so-called relative jet velocity distribution. 3. For passenger side airbags the cone is replaced by a wedge type shape. The first and secondary jet focal points define the corners of the wedge and the angle 𝛼 then defines the wedge angle. 4. Instead of applying pressure to all surfaces in the line of sight of the virtual origin(s), a part set can be defined to which the pressure is applied. 5. Care must be used to place the jet focal point within the bag. If the focal point is outside the bag, inside surfaces will not be visible so jetting pressure will not be applied correctly. Additional card required for CM option: The following additional card is defined for the WANG_NEFSKE_JETTING_CM and WANG_NEFSKE_MULTIPLE_JETTING_CM options. Additional card required for CM keyword option. Card 10 1 2 3 4 5 6 7 8 Variable NREACT Type I Default none Remark VARIABLE NREACT Remarks: DESCRIPTION Node for reacting jet force. If zero the jet force will not be applied. Compared with the standard LS-DYNA jetting formulation, the Constant Momentum option has several differences. Overall, the jetting usually has a more significant effect on airbag deployment than the standard LS-DYNA jetting: the total force is often greater, and does not reduce with distance from the jet. The velocity at the jet outlet is assumed to be a choked (sonic) adiabatic flow of a perfect gas. Therefore the velocity at the outlet is given by: 𝑣outlet = √𝛾𝑅𝑇 = √ (𝑐𝑝 − 𝑐𝑣)𝑇𝑐𝑝 𝑐𝑣 The density in the nozzle is then calculated from conservation of mass flow. 𝜌0𝜈outlet𝐴outlet = 𝑚̇ This is different from the standard LS-DYNA jetting formulation, which assumes that the density of the gas in the jet is the same as atmospheric air, and then calculates the jet velocity from conservation of mass flow. The velocity distribution at any radius, 𝑟, from the jet centerline and distance, 𝑧, from the focus, 𝑣𝑟,𝑧relates to the velocity of the jet centerline, 𝑣𝑟 = 0, 𝑧, in the same way as the standard LS-DYNA jetting options: 𝑣𝑟,𝑧 = 𝑣𝑟=0,𝑧𝑒−( 𝑟 𝛼𝑧) The velocity at the jet centerline, 𝑣𝑟 = 0, at the distance, 𝑧, from the focus of the jet is calculated such that the momentum in the jet is conserved. momentum at nozzle = momentum at z 𝜌0𝑣outlet 𝐴outlet = 𝜌0 ∫ 𝑣jet 2 𝑑𝐴jet = 𝜌0𝑣𝑟=0,𝑍 {𝑏 + 𝐹√𝑏} where, 𝑏 = 𝜋(𝛼𝑧)2 , and 𝐹 is the distance between the jet foci (for a passenger jet). Finally, the pressure exerted on an airbag element in view of the jet is given as: By combining the equations above 2 𝑝𝑟,𝑧 = 𝛽𝜌0𝑣𝑟,𝑧 𝑝𝑟,𝑧 = ] 𝛽𝑚̇ 𝑣outlet[𝑒−(𝑟/𝛼𝑧)2 {⎧𝜋(𝛼𝑧)2 ⎩{⎨ + 𝐹√𝜋(𝛼𝑧)2 }⎫ ⎭}⎬ The total force exerted by the jet is given by 𝐹jet = 𝑚̇ 𝑣outlet, which is independent of the distance from the nozzle. Mass flow in the jet is not necessarily conserved, because gas is entrained into the jet from the surrounding volume. By contrast, the standard LS-DYNA jetting formulation conserves mass flow but not momentum. This has the effect of making the jet force reduce with distance from the nozzle. The jetting forces can be reacted onto a node (NREACT), to allow the reaction force through the steering column or the support brackets to be modeled. The jetting force is written to the ASCII abstat file and the binary xtf file. *AIRBAG Additional card required for LOAD_CURVE option. (For card 1 see the “core cards” section of *AIRBAG.) Card 2 1 2 Variable STIME LCID Type F I 3 RO F 4 PE F 5 P0 F 6 T F 7 T0 F 8 Default 0.0 none none none none none none VARIABLE DESCRIPTION Time at which pressure is applied. The load curve is offset by this amount. Load curve ID defining pressure versus time, see *DEFINE_- CURVE. Initial density of gas (ignored if LCID > 0) Ambient pressure (ignored if LCID > 0) Initial gauge pressure (ignored if LCID > 0) Gas Temperature (ignored if LCID > 0) Absolute zero on temperature scale (ignored if LCID > 0) STIME LCID RO PE P0 T T0 Remarks: Within this simple model the control volume is inflated with a pressure defined as a function of time or calculated using the following equation if LCID = 0. 𝑃total = 𝐶𝜌(𝑇 − 𝑇0) 𝑃gauge = 𝑃total − 𝑃ambient The pressure is uniform throughout the control volume. *AIRBAG_LINEAR_FLUID Additional card required for LINEAR_FLUID option. (For card 1 see the “core cards” section of *AIRBAG.) Card 2 1 Variable BULK Type F 2 RO F 3 4 5 6 7 8 LCINT LCOUTT LCOUTP LCFIT LCBULK LCID I I I I I I Default none none none optional optional optional optional none Card 3 is optional. Card 3 1 2 3 4 5 6 7 8 Variable P_LIMIT P_LIMLC Type F I Default optional optional VARIABLE BULK DESCRIPTION K, bulk modulus of the fluid in the control volume. Constant as a function of time. Define if LCBULK = 0. RO 𝜌, density of the fluid LCINT LCOUTT LCOUTP LFIT 𝐹(𝑡) input flow curve defining mass per unit time as a function of time, see *DEFINE_CURVE. 𝐺(𝑡), output flow curve defining mass per unit time as a function of time. This load curve is optional. 𝐻(𝑝), output flow curve defining mass per unit time as a function of pressure. This load curve is optional. 𝐿(𝑡), added pressure as a function of time. This load curve is optional. VARIABLE LCBULK DESCRIPTION Curve defining the bulk modulus as a function of time. This load curve is optional, but if defined, the constant, BULK, is not used. LCID Load curve ID defining pressure versus time, see *DEFINE_- CURVE. P_LIMIT Limiting value on total pressure (optional). P_LIMLC Curve defining the limiting pressure value as a function of time. If nonzero, P_LIMIT is ignored. Remarks: If LCID = 0 then the pressure is determined from: 𝑃(𝑡) = 𝐾(𝑡)ln [ 𝑉0(𝑡) 𝑉(𝑡) ] + 𝐿(𝑡). where, 𝑃(𝑡) = Pressure, 𝑉(𝑡) = Volume of fluid in compressed state, 𝑉0(𝑡) = 𝑉0(𝑡) = 𝑀(𝑡) = Volume of fluid in uncompressed state, 𝑀(𝑡) = 𝑀(0) + ∫ 𝐹(𝑡)𝑑𝑡 − ∫ 𝐺(𝑡)𝑑𝑡 − ∫ 𝐻(𝑝)𝑑𝑡 = Current fluid mass, 𝑀(0) = 𝑉(0)𝜌 = Mass of fluid at time zero 𝑃(0) = 0. By setting LCID ≠ 0 a pressure time history may be specified for the control volume and the mass of fluid within the volume is then calculated from the volume and density. This model is for the simulation of hydroforming processes or similar problems. The pressure is controlled by the mass flowing into the volume and by the current volume. The pressure is uniformly applied to the control volume. Note the signs used in the equation for 𝑀(𝑡). The mass flow should always be defined as positive since the output flow is subtracted. *AIRBAG_HYBRID_OPTIONS *AIRBAG_HYBRID_JETTING_OPTIONS Additional cards required for HYBRID and HYBRID_JETTING options. (For card 1 see the “core cards” section of *AIRBAG.) Card 2 1 2 3 4 5 6 7 8 Variable ATMOST ATMOSP ATMOSD GC CC HCONV Type F F F F F F Default none none none none 1.0 none Card 3 1 2 3 4 5 6 7 8 Variable C23 LCC23 A23 LCA23 CP23 LCP23 AP23 LCAP23 Type F Default none Card 4 1 I 0 2 F none 3 I 0 4 F none 5 I 0 6 F none 7 I 0 8 Variable OPT PVENT NGAS LCEFR LCIDM0 VNTOPT Type I F I Default none none none I 0 I 0 I Include NGAS pairs of cards 5 and 6: Card 5 1 2 3 4 5 Variable LCIDM LCIDT MW INITM Type I I F F 6 A F 7 B F 8 C F Default none none none none none none none Card 6 1 2 3 4 5 6 7 8 Variable FMASS Type F Default none VARIABLE DESCRIPTION ATMOST Atmospheric temperature ATMOSP Atmospheric pressure ATMOSD Atmospheric density GC CC HCONV Universal molar gas constant Conversion constant EQ.0: Set to 1.0. Effective heat transfer coefficient between the gas in the air bag and the environment at temperature at ATMOST. If HCONV < 0, then HCONV defines a load curve of data pairs (time, hconv). C23 Vent orifice coefficient which applies to exit hole. Set to zero if LCC23 is defined below. LCC23 A23 LCA23 CP23 LCCP23 *AIRBAG_HYBRID DESCRIPTION The absolute value, |LCC23|, is a load curve ID. If the ID is positive, the load curve defines the vent orifice coefficient which applies to exit hole as a function of time. If the ID is negative, the vent orifice coefficient is defined as a function of relative pressure, 𝑃air/𝑃bag, see [Anagonye and Wang 1999]. In addition, LCC23 can be defined through *DEFINE_CURVE_FUNCTION. A nonzero value for C23 overrides LCC23 If defined as a positive number, A23 is the vent orifice area which applies to exit hole. If defined as a negative number, the absolute value |A23| is a part ID, see [Anagonye and Wang 1999]. The area of this part becomes the vent orifice area. Airbag pressure will not be applied to part |A23| representing venting holes if part |A23| is not included in SID, the part set representing the airbag. Set A23 to zero if LCA23 is defined below. Load curve number defining the vent orifice area which applies to exit hole as a function of absolute pressure, or LCA23 can be defined through *DEFINE_CURVE_FUNCTION. A nonzero value for A23 overrides LCA23. Orifice coefficient for leakage (fabric porosity). Set to zero if LCCP23 is defined below. Load curve number defining the orifice coefficient for leakage (fabric porosity) as a function of time, or LCCP23 can be defined through *DEFINE_CURVE_FUNCTION. A nonzero value for CP23 overrides LCCP23. AP23 Area for leakage (fabric porosity) LCAP23 Load curve number defining the area for leakage (fabric porosity) as a function of (absolute) pressure, or LCAP23 can be defined through *DEFINE_CURVE_FUNCTION. A nonzero value for AP23 overrides LCAP23. VARIABLE OPT DESCRIPTION Fabric venting option, if nonzero CP23, LCCP23, AP23, and LCAP23 are set to zero. EQ.1: Wang-Nefske formulas for venting through an orifice are used. Blockage is not considered. EQ.2: Wang-Nefske formulas for venting through an orifice are used. Blockage of venting area due to contact is consid- ered. EQ.3: Leakage formulas of Graefe, Krummheuer, and Siejak [1990] are used. Blockage is not considered. EQ.4: Leakage formulas of Graefe, Krummheuer, and Siejak [1990] are used. Blockage of venting area due to contact is considered. EQ.5: Leakage formulas based on flow through a porous media are used. Blockage due to contact is not considered. EQ.6: Leakage formulas based on flow through a porous media are used. Blockage due to contact is considered. EQ.7: Leakage is based on gas volume outflow versus pressure load curve. Blockage of flow area due to contact is not considered. Absolute pressure is used in the porous- velocity-versus-pressure load curve, given as FAC(𝑃) in the *MAT_FABRIC card. EQ.8: Leakage is based on gas volume outflow versus pressure load curve. Blockage of flow area due to contact is con- sidered. PVENT Gauge pressure when venting begins NGAS LCEFR LCIDM0 Number of gas inputs to be defined below (Including initial air). The maximum number of gases is 17. Optional curve for exit flow rate (mass/time) versus (gauge) pressure Optional curve representing inflator’s total mass inflow rate. When defined, LCIDM in the following 2 × NGAS cards defines the molar fraction of each gas component as a function of time and INITM defines the initial molar ratio of each gas component. *AIRBAG_HYBRID DESCRIPTION VNTOPT Additional options for venting area definition. For A23 ≥ 0 EQ.1: Vent area is equal to A23. EQ.2: Vent area is A23 plus the eroded surface area of the airbag parts. EQ.10: Same as VNTOPT = 2 For A23 < 0 EQ.1: Vent area is the increase in surface area of part |A23|. If there is no change in surface area of part |A23| over the initial surface area or if the surface area reduces from the initial area, there is no venting. EQ.2: Vent area is the total (not change in) surface area of part |A23| plus the eroded surface area of all other parts comprising the airbag. EQ.10: Vent area is the increase in surface area of part |A23| plus the eroded surface area of all other parts compris- ing the airbag. LCIDM Load curve ID for inflator mass flow rate (eq. 0 for gas in the bag at time = 0) GT.0: piecewise linear interpolation LT.0: cubic spline interpolation LCIDT Load curve ID for inflator gas temperature (eq.0 for gas in the bag at time 0) GT.0: piecewise linear interpolation LT.0: cubic spline interpolation MW Molecular weight INITM Initial mass fraction of gas component present in the airbag, prior to injection of gas by the inflator A B Coefficient for molar heat capacity of inflator gas at constant pressure, (e.g., Joules/mole/oK) Coefficient for molar heat capacity of inflator gas at constant pressure, (e.g., Joules/mole/oK2) VARIABLE DESCRIPTION C Coefficient for molar heat capacity of inflator gas at constant pressure, (e.g., Joules/mole/oK3) FMASS Fraction of additional aspirated mass. Aditional cards are required for HYBRID_JETTING and HYBRID_JETTING_CM The following two additional cards are defined for the HYBRID_JETTING options. The jet may be defined by specifying either the coordinates of the jet focal point, jet vector head and secondary jet focal point, or by specifying three nodes located at these positions. The nodal point option is recommended when the location of the airbag changes as a function of time. Card 7 1 2 3 4 5 6 Variable XJFP YJFP ZJFP XJVH YJVH ZJVH Type F F F F F F 7 CA F 8 BETA F Default none none none none none none none none Remark 1 Card 8 1 1 2 1 3 1 4 1 5 1 6 7 8 Variable XSJFP YSJFP ZSJFP PSID IDUM NODE1 NODE2 NODE3 Type F F F I F Default none none none none none Remark 2 I 0 1 I 0 1 I 0 Additional card required for HYBRID_JETTING_CM option. Card 9 1 2 3 4 5 6 7 8 Variable NREACT Type I Default none Remark 4 VARIABLE DESCRIPTION XJFP YJFP ZJFP XJVH YJVH ZJVH CA 𝑥-coordinate of jet focal point, i.e., the virtual origin in Figures 3-1 and 3-2. See Remark 1 below. 𝑦-coordinate of jet focal point, i.e., the virtual origin in Figures 3-1 and 3-2. 𝑧-coordinate of jet focal point, i.e., the virtual origin in Figures 3-1 and 3-2. 𝑥-coordinate of jet vector head to defined code centerline 𝑦-coordinate of jet vector head to defined code centerline 𝑧-coordinate of jet vector head to defined code centerline Cone angle, 𝛼, defined in radians. LT.0.0: |𝛼| is the load curve ID defining cone angle as a function of time BETA Efficiency factor, 𝛽, which scales the final value of pressure obtained from Bernoulli’s equation. LT.0.0: ∣𝛽∣ is the load curve ID defining the efficiency factor as a function of time XSJFP 𝑥-coordinate of secondary jet focal point, passenger side bag. If the coordinate of the secondary point is (0,0,0) then a conical jet (driver’s side airbag) is assumed. YSJFP 𝑦-coordinate of secondary jet focal point VARIABLE DESCRIPTION ZSJFP PSID 𝑧-coordinate of secondary jet focal point Optional part set ID, see *SET_PART. If zero all elements are included in the airbag. IDUM Dummy field (Variable not used) NODE1 Node ID located at the jet focal point, i.e., the virtual origin in Figure 3-7. See Remark 1 below. NODE2 Node ID for node along the axis of the jet. NODE3 Optional node ID located at secondary jet focal point. NREACT Node for reacting jet force. If zero the jet force will not be applied. Remarks: 1. Jetting. It is assumed that the jet direction is defined by the coordinate method (XJFP, YJFP, ZJFP) and (XJVH, YJVH, ZJVH) unless both NODE1 and NODE2 are defined. In which case the coordinates of the nodes given by NODE1, and NODE2 (XJVH, YJVH, ZJVH). The use of nodes is recommended if the airbag system is undergoing rigid body motion. The nodes should be attached to the vehicle to allow for the coordinates of the jet to be continuously updated with the motion of the vehicle. and NODE3 will (XJFP, YJFP, ZJFP) override The jetting option provides a simple model to simulate the real pressure distri- bution in the airbag during the breakout and early unfolding phase. Only the surfaces that are in the line of sight to the virtual origin have an increased pres- sure applied. With the optional load curve LCRJV, the pressure distribution with the code can be scaled according to the so-called relative jet velocity distri- bution. For passenger side airbags the cone is replaced by a wedge type shape. The first and secondary jet focal points define the corners of the wedge and the angle 𝛼 then defines the wedge angle. Instead of applying pressure to all surfaces in the line of sight of the virtual origin(s), a part set can be defined to which the pressure is applied. 2. IDUM. This variable is not used and has been included to maintain the same format as the WANG_NEFSKE_JETTING options. 3. Focal Point Placement. Care must be used to place the jet focal point within the bag. If the focal point is outside the bag, inside surfaces will not be visible so jetting pressure will not be applied correctly. 4. NREACT. See the description related to the WANG_NEFSKE_JETTING_CM option. For the hybrid inflator model the heat capacities are compute from the combination of gases which inflate the bag. *AIRBAG_HYBRID_CHEMKIN_OPTION The HYBRID_CHEMKIN model includes 3 control cards. For each gas species an additional set of cards must follow consisting of a control card and several thermodynamic property data cards. (For card 1 see the “core cards” section of *AIRBAG.) Card 2 1 2 3 4 5 6 Variable LCIDM LCIDT NGAS DATA ATMT ATMP Type I I I I F F 8 7 RG F Default none none none none none none none Card 3 1 2 3 4 5 6 7 8 Variable HCONV Type F Default 0. Card 4 1 2 3 4 5 6 7 8 Variable C23 A23 Type F Default 0. F 0. VARIABLE DESCRIPTION LCIDM Load curve specifying input mass flow rate versus time. GT.0: piece wise linear interpolation LT.0: cubic spline interpolation *AIRBAG_HYBRID_CHEMKIN DESCRIPTION LCIDT Load curve specifying input gas temperature versus time. GT.0: piece wise linear interpolation LT.0: cubic spline interpolation NGAS DATA Number of gas inputs to be defined below. (Including initial air) Thermodynamic database EQ.1: NIST database (3 additional property cards are required below) EQ.2: CHEMKIN database (no additional property cards are required) EQ.3: Polynomial data (1 additional property card is required below) ATMT ATMP Atmospheric temperature. Atmospheric pressure RG Universal gas constant HCONV Effective heat transfer coefficient between the gas in the air bag and the environment at temperature ATMT. If HCONV < 0, then HCONV defines a load curve of data pairs (time, hconv). C23 A23 Vent orifice coefficient Vent orifice area NGAS Sets of Gas Species Data Cards: For each gas species include a set of cards consisting of a Gas Species Control Card followed by several thermo-dynamic property data cards whose format depends on the DATA parameter on card in format “card 5”. The next "*" card terminates the reading of this data. Gas Species Control Card. Card 5 1 2 3 4 5 6 7 8 Variable CHNAME MW LCIDN FMOLE FMOLET Type A F Default none none I 0 F F none 0. VARIABLE CHNAME DESCRIPTION Chemical symbol for this gas species (e.g., N2 for nitrogen, AR for argon). Required for DATA = 2 (CHEMKIN), optional for DATA = 1 or DATA = 3. MW Molecular weight of this gas species. LCIDN Load curve specifying the input mole fraction versus time for this gas species. If > 0, FMOLE is not used. FMOLE Mole fraction of this gas species in the inlet stream. FMOLET Initial mole fraction of this gas species in the tank. Additional thermodynamic data cards for each gas species. If DATA = 1, include the following 3 cards for the NIST database: The required data can be found on the NIST web site at http://webbook.nist.gov/ chemistry/. Card 5a 1 2 3 4 5 6 7 8 Variable TLOW TMID THIGH Type F F F Default none none none Card 5b 1 2 3 4 5 6 7 8 Variable alow blow clow dlow elow flow hlow Type F F F F F F F Default none none none none none none none Card 5c 1 2 3 4 5 6 7 8 Variable ahigh bhigh chigh dhigh ehigh fhigh hhigh Type F F F F F F F Default none none none none none none none VARIABLE DESCRIPTION TLOW TMID Curve fit low temperature limit. Curve fit low-to-high transition temperature. THIGH Curve fit high temperature limit. VARIABLE alow, …, hlow DESCRIPTION Low temperature range NIST polynomial curve fit coefficients . ahigh, …, hhigh High temperature range NIST polynomial curve fit coefficients . No additional cards are needed if using the CHEMKIN database (DATA = 2): 6 7 8 Polynomial Fit Card (DATA = 3). Card 5d Variable Type 1 a F 2 b F 3 c F 4 d F 5 e F Default none 0. 0. 0. 0. VARIABLE DESCRIPTION a b c d e Coefficient, see below. Coefficient, see below. Coefficient, see below. Coefficient, see below. Coefficient, see below. Specific heat curve fits: NIST: 𝑐𝑝 = CHEMKIN: 𝑐𝑝 = POLYNOMIAL: 𝑐𝑝 = (𝑎 + 𝑏𝑇 + 𝑐𝑇2 + 𝑑𝑇3 + 𝑇2) (𝑎 + 𝑏𝑇 + 𝑐𝑇2 + 𝑑𝑇3 + 𝑒𝑇4) (𝑎 + 𝑏𝑇 + 𝑐𝑇2 + 𝑑𝑇3 + 𝑒𝑇4) 𝑅̅̅̅̅̅ 𝑅̅̅̅̅̅ = universal gas constant 8.314 Nm mole × 𝐾 where, 𝑀 = gas molecular weight *AIRBAG_FLUID_AND_GAS_OPTIONS Additional cards required for FLUID_AND_GAS option. (For card 1 see the “core cards” section of *AIRBAG.) Currently this option only works in SMP and explicit analysis. Card 2 1 2 3 Variable XWINI XWADD XW Type F F F 4 P F 5 6 7 8 TEND RHO LCXW LCP F F I I Default none none none none none none none none Card 3 1 2 3 4 5 6 7 8 Variable GDIR NPROJ IDIR IIDIR KAPPA KBM Type F Default none I 3 I I F F none none 1.0 none VARIABLE DESCRIPTION XWINI Fluid level at time 𝑡 = 0 in |GDIR| direction. XWADD Fluid level filling increment per time step. XW P Final fluid level in filling process. Gas pressure at time 𝑡 = TEND. TEND Time when gas pressure P is reached. RHO LCXW LCP Density of the fluid (e.g. for water, RHO ≈ 1.0 kg/m3) Load curve ID for fluid level vs. time. XW, XWADD, and XWINI are with this option. Load curve ID for gas pressure vs. time. P and TEND are ignored with this option. GDIR *AIRBAG_FLUID_AND_GAS DESCRIPTION Global direction of gravity (e.g. -3.0 for negative global z-axis). EQ.1.0: global 𝑥-direction, EQ.2.0: global 𝑦-direction, EQ.3.0: global 𝑧-direction. NPROJ IDIR IIDIR Number of projection directions (only global axis) for volume calculation. First direction of projection (if ∣NPROJ∣ ≠ 3), only global axis. Second direction of projection (if |NPROJ| = 2), only global axis. KAPPA Adiabatic exponent KBM Bulk modulus of the fluid (e.g. for water, BKM ≈ 2080 N/mm2) Remarks: The *AIRBAG_FLUID_AND_GAS option models a quasi-static multi chamber fluid/gas structure interaction in a simplified way including three possible load cases: (i) only gas, (ii) only incompressible fluid, or (iii) the combination of incompressible fluid with additional gas “above”. see Figure 3-5. Figure 3-5. Hydrostatic pressure distribution in a chamber filled with gas and incompressible fluid The theory is based on the description of gases and fluids as energetically equivalent pressure loads. The calculation of the fluid volume is carried out using the directions of projection and a non-normalized normal vector. This model, therefore, requires that the normal of the shell elements belonging to a filled structure must point outwards. Holes are not detected, but can be taken into account as described below. In case of a pure gas (no fluid), the *AIRBAG_SIMPLE_PRESSURE_VOLUME and *AIRBAG_FLUID_AND_GAS cards give identical results as they are based on the same theory. The update of the gas pressure due to volume change is calculated with the following simple gas law 𝑝𝑔 = ⎜⎛1 − KAPPA × ⎝ 𝑣𝑔 − 𝑣old 𝑣old 𝑔 ⎟⎞ 𝑝old ⎠ with adiabatic exponent KAPPA and gas volume 𝑣𝑔. The theory of incompressible fluids is based on the variation of the potential energy and an update of the water level due to changes in the volume and the water surface, see Haßler and Schweizerhof [2007], Haßler and Schweizerhof [2008], Rumpel and Schweizerhof [2003], and Rumpel and Schweizerhof [2004]. In case of multiple fluid/gas filled chambers each chamber requires an additional *AIRBAG_FLUID_AND_GAS card. Some of the parameters which are called local parameters only belong to a single chamber (e.g. gas pressure). In contrast global, parameters belong to all chambers (e.g. direction of gravitation). Because the theory only applies to quasi-static fluid-structure interaction the load has to be applied slowly so that the kinetic energy is almost zero throughout the process. All parameters of card 1 are local parameters describing the filling of the chamber. The water level and the gas pressure can be defined by curves using LCXW and LCP. A second possibility are the parameters XWINI, XW, XWADD, P and TEND. When describing the fluid and gas filling using the parameters the gas pressure at time 𝑡 = 0 is set to 0 and the initial water level is set to XWINI in |GDIR|-direction. At each timestep, XWADD is added to the water level, until XW is reached. The gas pressure will be raised until P is reached at time 𝑡 = TEND. In general, global parameters belong to all chambers. To describe the global axis in GDIR, NPROJ, IDIR and IIDIR the following relations apply: 𝑥-axis is axis “1”, the 𝑦- axis is axis “2”, and the 𝑧-axis is axis 3. The gas and fluid volume is calculated by contour integrals in the global 𝑥-, 𝑦- and 𝑧- coordinates. If one of the boundaries is discontinuous in one or two global directions, these directions have to be ignored in NPROJ, IDIR and IIDIR. At least one direction of projection must be set (NPROJ = 1, IDIR = value), but it is recommended to use as many directions of projection as possible. In case of a structure filled exclusively with fluid, IDIR and IIDIR should not be set to |GDIR|. In case of holes in a structure (e.g. to take advantage of symmetry planes), IDIR and IIDIR should not be set to the normal direction of the plane describing the hole or symmetry plane. An example of a water filled tube structure illustrating how to use NPROJ, IDIR, IIDIR, and GDIR is shown in Figure 3-6. In this example gravity is acting opposite to the global 𝑧-axis. In this case, then, GDIR = -3. The structure is filled exclusively with water, so the projection direction cannot be set to |GDIR| = 3. To use the symmetry of the tube only half of the structure has been modeled. The normal of the symmetry plane shows in 𝑦 direction, so the projection direction cannot be set to 2. Because the symmetry axes (2 and 3) are not allowed, the only direction of projection is 1; therefore, NPROJ = 1 and IDIR = 1. Figure 3-6. Example for water filled tube structure For further explanations and examples see Haßler and Schweizerhof [2007], Haßler and Schweizerhof [2008], and Maurer, Gebhardt, and Schweizerhof [2010]. The possible entries for NPROJ, IDIR and IIDIR are: NPROJ IDIR IIDIR 3 2 2 2 1 1 1 2 3 3 1 1 2 1 2 *AIRBAG Purpose: The input in this section provides a simplified approach to defining the deployment of the airbag using the ALE capabilities with an option to switch from the initial ALE method to control volume (CV) method (*AIRBAG_HYBRID) at a chosen time. An enclosed airbag (and possibly the airbag canister/compartment and/or a simple representation of the inflator) shell structure interacts with the inflator gas(es). This definition provides a single fluid to structure coupling for the airbag-gas interaction during deployment in which the CV input data may be used directly. Card 1 1 2 3 4 5 6 7 8 Variable SID SIDTYP MWD SPSF Type I I Default none none F 0 F 0 Remark 1 VARIABLE SID DESCRIPTION Set ID as defined on *AIRBAG card. This set ID contains the Lagrangian elements (segments) which make up the airbag and possibly the airbag canister/compartment and/or a simple representation of the inflator. See Remark 1. SIDTYP Set type: EQ.0: Segment set. EQ.1: Part set. MWD SPSF Mass weighted damping factor, D. This is used during the CV phase for *AIRBAG_HYBRID. Stagnation pressure scale factor, 0 ≤ 𝛾 ≤ 1. This is used during the CV phase for *AIRBAG_HYBRID. Card 2 1 2 3 Variable ATMOST ATMOSP Type F Default 0. Remark 2 F 0. 2 *AIRBAG_ALE 4 GC F 5 6 7 8 CC TNKVOL TNKFINP F F F none 1.0 0.0 0.0 10 10 VARIABLE DESCRIPTION ATMOST Atmospheric ambient temperature. See Remark 2. ATMOSP Atmospheric ambient pressure. See Remark 2. GC CC TNKVOL Universal molar gas constant. Conversion constant. If EQ: .0 Set to 1.0. Tank volume from the inflator tank test or Inflator canister volume. See remark 10. LCVEL = 0 and TNKFINP is defined: TNKVOL is the defined Tank. Inlet gas velocity is estimat- ed by LS-DYNA method (testing). LCVEL = 0 and TNKFINP is not defined TNKVOL is the estimated inflator canister volume Inlet gas velocity is estimated automatically by the Lian- Bhalsod-Olovsson method. LCVEL ≠ 0 This must be left blank. TNKFINP Tank final pressure from the inflator tank test data. Only define this parameter for option 1 of TNKVOL definition above. See Remark 10. Coupling Card. See keyword *CONSTRAINED_LAGRANGE_IN_SOLID. Card 3 1 2 3 4 5 6 7 8 Variable NQUAD CTYPE PFAC FRIC FRCMIN NORMTYP ILEAK PLEAK Type Default I 4 I 4 F F F 0.1 0.0 0.3 I 0 I 2 F 0.1 Remark 13 13 14 VARIABLE NQUAD DESCRIPTION Number of (quadrature) coupling points for coupling Lagrangian slave parts to ALE master solid parts. If NQUAD = n, then nXn coupling points will be parametrically distributed over the surface of each Lagrangian slave segment (default = 4). See Remark 13. CTYPE Coupling type (default = 4, see Remark 13): PFAC EQ.4: (default) penalty coupling with DIREC = 2 implied. EQ.6: penalty coupling in which DIREC is automatically set to DIREC = 1 for the unfolded region and DIREC = 2 for folded region. Penalty factor. PFAC is a scale factor for scaling the estimated stiffness of the interacting (coupling) system. It is used to compute the coupling forces to be distributed on the slave and master parts. GT.0: Fraction of estimated critical stiffness (default = 0.1). LT.0: -PFAC is a load curve ID. The curve defines the relative coupling pressure (y-axis) as a function of the tolerable fluid penetration distance (x-axis). FRIC Coupling coefficient of friction. FRCMIN Minimum fluid volume fraction in an ALE element to activate coupling (default is 0.3). *AIRBAG_ALE DESCRIPTION NORMTYP Penalty coupling spring direction (DIREC 1 and 2): EQ.0: normal vectors are interpolated from nodal normals (default) EQ.1: normal vectors are interpolated from segment normals. ILEAK Leakage control flag. Default = 2 (with energy compensation). PLEAK Leakage control penalty factor (default = 0.1) Venting Hole Card. Card 4 1 2 3 4 5 6 7 8 Variable IVSETID IVTYPE IBLOCK VNTCOF Type Default Remark I 0 4 I 0 I 0 5 F 0.0 6 VARIABLE DESCRIPTION IVSETID Set ID defining the venting hole surface(s). See Remark 4. IVTYPE Set type of IVSETID: EQ.0: Part Set (default). EQ.1: Part ID. EQ.2: Segment Set. IBLOCK Flag for considering blockage effects for porosity and vents : EQ.0: no (blockage is NOT considered, default). EQ.1: yes (blockage is considered). VNTCOF Vent Coefficient for scaling the flow. See Remark 6. transformation. Parameters for ALE mesh automatic definition and its *AIRBAG Card 5 1 2 3 4 5 6 7 8 Variable NX/IDA NY/IDG NZ MOVERN ZOOM Type I I I Default none none none Remark 7 7 7 I 0 8 I 0 9 VARIABLE DESCRIPTION Option 1: Automatic ALE mesh, activated by NZ.NE.0 (blank): NX NY NZ NX is the number of ALE elements to be generated in the x direction. See remark 7. NY is the number of ALE elements to be generated in the y direction. See remark 7. NZ is the number of ALE elements to be generated in the z direction. See remark 7. Option 2: ALE mesh from part ID: IDAIR IDAIR is the Part ID of the initial air mesh. See remark 7. IDGAS IDGAS is defined as Part ID of the initial gas mesh. See remark 7. NZ Leave blank to activate options 2. See remark 7. Variables common to both options: MOVERN ALE mesh automatic motion option . EQ.0: ALE mesh is fixed in space. GT.0: Node group id. See *ALE_REFERENCE_SYSTEM_- NODE ALE mesh can be moved with PRTYP = 5, mesh motion follows a coordinate system defined by 3 refer- ence nodes. *AIRBAG_ALE DESCRIPTION ZOOM ALE mesh automatic expansion option : EQ.0: do not expand ALE mesh EQ.1: Expand/contract ALE mesh by keeping all airbag parts to the ALE mesh (equivalent contained within PRTYP = 9). Origin for ALE Mesh Card. Include Cards 5a and 5b when NZ > 0. Card 5a Variable 1 X0 Type F 2 Y0 F 3 Z0 F 4 X1 F 5 Y1 F 6 Z1 F 7 8 Default none none none none none none Card 5b Variable 1 X2 Type F 2 Y2 F 3 Z2 F 4 Z3 F 5 Y3 F 6 Z3 F 7 8 Default none none none none none none VARIABLE DESCRIPTION X0, Y0, Z0 Coordinates of origin for ALE mesh generation (node0). X1, Y1, Z1 Coordinates of point 1 for ALE mesh generation (node1). 𝑥-extent = node1 − node0 X2, Y2, Z2 Coordinates of point 2 for ALE mesh generation (node2). 𝑦-extent = node2 − node0 X3, Y3, Z3 Coordinates of point 3 for ALE mesh generation(node3). 𝑧-extent = node3 − node0 (x4, y4, z4) (x1, y1, z1) (x2, y2, z2) ( = y(=3) ) (x0, y0, z0) 8 ) x( = Figure 3-7. Illustration of automatic mesh generation for the ALE mesh in a hexahederal region Miscellaneous Parameters Card. 3 HG F 0. 4 5 6 7 8 NAIR NGAS NORIF LCVEL LCT I 0 I 0 I 0 I 0 I 0 10 11 Card 6 1 2 Variable SWTIME Type F Default 1e16 Remarks 3 VARIABLE SWTIME DESCRIPTION Time to switch from ALE method to control volume (CV) method. Once switched, a method similar to that used by the *AIRBAG_HYBRID card is used. HG NAIR Hourglass control for ALE fluid mesh(es). Number of Air components. For example, this equals 2 in case air contains 80% of N2 and 20% of O2. If air is defined as 1 single gas then NAIR = 1. NGAS Number of inflator Gas components. NORIF LCVEL *AIRBAG_ALE DESCRIPTION Number of point sources or orifices. This determines the number of point source cards to be read. Load curve ID for inlet velocity . This is the same estimated velocity curve used in *SECTION_POINT_SOURCE_MIXTURE card. LCT Load curve ID for inlet gas temperature . Air Component Card. Include NAIR cards, one for each air component. Card 7 1 2 3 4 5 6 7 8 Variable Type Default Remarks MWAIR INITM AIRA AIRB AIRC F 0 F 0 F 0 F 0. F 0. 12 12 12 VARIABLE DESCRIPTION MWAIR Molecular weight of air component INITA AIRA AIRB AIRC Initial Mass Fraction of Air component(s) First Coefficient of molar heat capacity at constant pressure (e.g., J/mole/K, remark 12). Second Coefficient of molar heat capacity at constant pressure (e.g., J/mole/K2, remark 12). Third Coefficient of molar heat capacity at constant pressure (e.g., J/mole/K3, remark 12). Gas Component Card. Include NGAS cards, one for each gas component. Card 8 1 2 3 4 5 6 7 8 Variable LCMF MWGAS GASA GASB GASC Type I Default none F 0 F 0 F 0. F 0. Remarks 11 12 12 12 VARIABLE LCMF DESCRIPTION Load curve ID for mass flow rate . MWGAS Molecular weight of inflator gas components. GASA GASB GASC First Coefficient of molar heat capacity at constant pressure (e.g., J/mole/K, remark 12). Second Coefficient of molar heat capacity at constant pressure (e.g., J/mole/K2, remark 12). Third Coefficient of molar heat capacity at constant pressure (e.g., J/mole/K3, remark 12). Point Source Cards. Include NORIF cards, one for each point source. Card 9 1 2 3 4 5 6 7 8 Variable NODEID VECID ORIFARE Type Default I 0 I 0 I 0 VARIABLE DESCRIPTION NODEID The node ID defining the point source. *AIRBAG_ALE DESCRIPTION VECID The vector ID defining the direction of flow at the point source. ORIFARE The orifice area at the point source. Remarks: 1. This set ID typically contains the Lagrangian segments of the 3 parts that are coupled to the inflator gas: airbag, airbag canister (compartment), inflator. As in all control-volume, orientation of elements representing bag and canister should point outward. During the ALE phase the segment normal will be re- versed automatically for fluid-structure coupling. However, the orientation of inflator element normal vectors should point to its center. See Figure 3-8. Bag fabric Inflator Canister Figure 3-8. Arrows indicate “outward” normal 2. Atmospheric density for the ambient gas (air) can be computed from 𝜌amb = 𝑃amb 𝑅𝑇amb 3. Since ALL ALE related activities will be turned off after the switch from ALE method to control-volume method, no other ALE coupling will exist beyond t = SWTIME. 4. Vent definition will be used for ALE venting. Upon switching area of the segments will be used for venting as a23 in *AIRBAG_HYBRID. 5. Fabric porosity for ALE and *AIRBAG_HYBRID can be defined on MAT_FAB- RIC. Define FLC and FAC on *MAT_FABRIC. FVOPT 7 and 8 will be used for both ALE and *AIRBAG_HYBRID. IBLOCK = 0 will use FVOPT = 7 and IBLOCK = 1 will use FVOPT = 8. 6. VCOF will be used to scale the vent area for ALE venting and this coefficient will be used as vent coefficient c23 for *AIRBAG_HYBRID upon switching. 7. 8. If NX, NY and NZ are defined (option 1), card 5a and card 5b should be defined to let LS-DYNA generate the mesh for ALE. Alternatively if NZ is 0 (option 2), then NX = IDAIR and NY = IDGAS. In the latter case the user need to supply the ALE mesh whose PID = IDAIR. If the airbag moves with the vehicle, set MOVERN = GROUPID, this GROUPID is defined using *ALE_REFERENCE_SYSTEM_NODE. The 3 nodes defined in ALE_REFERENCE_SYSTEM_NODE will be used to transform the ALE mesh. The point sources will also follow this motion. This simulates PRTYP = 5 in the *ALE_REFERENCE_SYSTEM_GROUP card. 9. Automatic expansion/contraction of the ALE mesh to follow the airbag expansion can be turned on by setting zoom = 1. This feature is particularly useful for fully folded airbags requiring very fine ale mesh initially. As the airbag inflates the ale mesh will be automatically scaled such that the airbag will be contained within the ALE mesh. This simulates PRTYP = 9 in the *ALE_REFERENCE_SYSTEM_GROUP card. 10. There are 3 methods for defining the inlet gas velocity: a) Inlet gas velocity is estimated by LSDYNA method (testing), if LCVEL = 0 ⇒ TNKVOL = Tank volume and TNKFINP = Tank final pressure from tank test data. b) Inlet gas velocity is estimated automatically by Lian-Bhalsod-Olovsson method if, LCVEL = 0 ⇒ TNKVOL = Tank volume. and TNKFINP = blank. c) Inlet gas velocity is defined by user via a load curve LCVEL if, LCVEL = n, TNKVOL = 0, and 11. LCT and LCIDM should have the same number of sampling points. TNKFINP = 0 12. The per-mass-unit, temperature-dependent, constant-pressure heat capacity is 𝐶𝑝(𝑇) = [𝐴 + 𝐵𝑇 + 𝐶𝑇2] 𝑀𝑊 . where, these quantities often have units of, 𝐴 = 𝐶̃𝑝0 𝐶𝑝(𝑇) kg × K 𝐶 mole × K mole × K2 mole × K3 13. Sometimes CTYPE = 6 may be used for complex folded airbag. NQUAD = 2 may be used as a starting value and increase as necessary depending on the relative mesh resolutions of the Lagrangian and ALE meshes. 14. Use a load curve for PFAC whenever possible. It tends to be more robust. Related Cards: AIR ⟶ GAS ⟶ {⎧*PART (AMMG2) *SECTION_SOLID ⎩{⎨ *MAT_GAS_MIXTURE {⎧*PART (AMMG1) *SECTION_POINT_SOURCE_MIXTURE ⎩{⎨ *MAT_GAS_MIXTURE Couplings ⟶ *CONSTRAINED_LAGRANGE_IN_SOLID ALE Mesh Motion ⟶ *ALE_REFERENCE_SYSTEM_GROUP Control Volume ⟶ *AIRBAG_HYBRID Vent ⟶ *AIRBAG_ALE/Card4 Example 1: $...|....1....|....2....|....3....|....4....|....5....|....6....|....7....|....8 *AIRBAG_ALE $#1 SID SIDTYPE NONE NONE NONE NONE MWD SPSF 123 1 0 0 0 0 0.0 0.0 $#2 ATMOST ATMOSP NONE GC CC TNKVOL TNKFP 298.15 1.0132E-4 0 8.314 0.0 0.0 0.0 $#3 NQUAD CTYPE PFAC FRIC FRCMIN NRMTYPE ILEAK PLEAK 4 4 -1000 0.0 0.3 0 2 0.1 $#4 VSETID IVSETTYP IBLOCK VENTCOEF 1 2 0 1.00 $#5NXIDAIR NYIDGAS NZ MOVERN ZOOM 50000 50003 0 0 0 $#6 SWTIME NONE HG NAIR NGAS NORIF LCVEL LCT 1000.00 0.000 1.e-4 1 1 8 2002 2001 $#7 AIR NONE NONE MWAIR INITM AIRA AIRB AIRC 0 0 0 0.02897 1.00 29.100 0.00000 0.00000 $#8 GASLCM NONE NONE MWGAS NONE GASA GASB GASC 2003 0 0 0.0235 0 28.000 0.00000 0.00000 $#9 NODEID VECTID ORIFAREA 100019 1 13.500000 100020 2 13.500000 100021 3 13.500000 100022 4 13.500000 100023 5 13.500000 100024 6 13.500000 100017 7 13.500000 100018 8 13.500000 $ PFAC CURVE = penalty factor curve. *DEFINE_CURVE $ lcid sidr sfa sfo offa offo dattyp 1000 0 0.0 2.0 0.0 0.0 $ a1 o1 0.0 0.00000000 1.0000000 4.013000e-04 *SET_SEGMENT_TITLE vent segments (defined in IVSETID) 1 0.0 0.0 0.0 0.0 1735 1736 661 1697 0.0 0.0 0.0 0.0 1735 2337 1993 1736 0.0 0.0 0.0 0.0 1735 1969 1988 2337 0.0 0.0 0.0 0.0 1735 1697 656 1969 0.0 0.0 0.0 0.0 *DEFINE_VECTOR $# vid xt yt zt xh yh zh 1 0.0 0.0-16.250000 21.213200 21.213200-16.250000 2 0.0 0.0-16.250000 30.000000-1.000e-06-16.250000 3 0.0 0.0-16.250000 21.213200-21.213200-16.250000 4 0.0 0.0-16.250000-1.000e-06-30.000000-16.250000 5 0.0 0.0-16.250000-21.213200-21.213200-16.250000 6 0.0 0.0-16.250000-30.0000001.0000e-06-16.250000 7 0.0 0.0-16.250000-21.213200 21.213200-16.250000 8 0.0 0.0-16.2500001.0000e-06 30.000000-16.250000 $...|....1....|....2....|....3....|....4....|....5....|....6....|....7....|....8 In this example, pre-existing background air mesh with part ID 50000 and gas mesh with part ID 50003 are used. Thus NZ = 0. There is no mesh motion nor expansion allowed. An inlet gas velocity curve is provided. Example 2: $...|....1....|....2....|....3....|....4....|....5....|....6....|....7....|....8 $ SIDTYP: 0=SGSID; 1=PSID *AIRBAG_ALE $#1 SID SIDTYPE NONE NONE NONE NONE MWD SPSF 1 1 0 0. 0. 0. 0. 0. $#2 ATMOST ATMOSP NONE GC CC TNKVOL TNKFP 298. 101325. 0.0 8.314 1. 6.0E-5 0 $#3 NQUAD CTYPE PFAC FRIC FRCMIN NRMTYPE ILEAK PLEAK 2 6 -321 0.0 0.3 1 2 0.1 $#4 VSETID IVSETTYP IBLOCK VENTCOEF 0 0 0 0 $#5NXIDAIR NYIDGAS NZ MOVERN ZOOM 11 11 9 $5b x0 y0 z0 x1 y1 z1 NOT-USED NOT-USED -0.3 -0.3 -0.135 0.3 -0.3 -0.135 $5c x2 y2 z2 x3 y3 z3 NOT-USED NOT-USED -0.3 0.3 -0.135 -0.3 -0.3 0.39 $#6 SWTIME NONE HG NAIR NGAS NORIF LCVEL LCT 0.04000 0.005 1.e-4 2 1 1 0 2 $#7 AIR NONE NONE MWAIR INITM AIRA AIRB AIRC 0.028 0.80 27.296 0.00523 0.032 0.20 25.723 0.01298 $#8 GASLCM NONE NONE MWGAS NONE GASA GASB GASC 1 0.0249 29.680 0.00880 $#9 NODEID VECTID ORIFAREA 9272 1 1.00e-4 $ Lagrangian shell structure to be coupled to the inflator gas *SET_PART_LIST 1 0.0 0.0 0.0 0.0 1 2 3 *DEFINE_VECTOR $0.100000E+01, 10.000000000 $ vid xt yt zt xh yh zh 1 0.0 0.0 0.0 0.0 0.0 0.100000 $ bag penetration ~ 1 mm <====> P_coup ~ 500000 pascal ==> ~ 5 atm *DEFINE_CURVE $ lcid sidr sfa sfo offa offo dattyp 321 0 0.0 0.0 0.0 0.0 $ a1 o1 0.0 0.0 0.00100000 5.0000000e+05 $...|....1....|....2....|....3....|....4....|....5....|....6....|....7....|....8 In this example, LS-DYNA automatically creates the background ALE mesh with: NX = 11 ⇒ 11 elements in the x direction NY = 11 ⇒ 11 Elements in the y direction NZ = 9 ⇒ 9 Elements in the z direction *AIRBAG Purpose: To define two connected airbags which vent into each other. Card 1 1 2 3 Variable AB1 AB2 AREA Type I I F 4 SF F Default none none none none 5 6 7 8 PID LCID IFLOW I 0 I 0 I 0 VARIABLE DESCRIPTION AB1 AB2 First airbag ID, as defined on *AIRBAG card. Second airbag ID, as defined on *AIRBAG card. AREA Orifice area between connected bags. LT.0.0: |AREA| is the load curve ID defining the orifice area as a function of absolute pressure. EQ.0.0: AREA is taken as the surface area of the part ID defined below. SF Shape factor. LT.0.0: |SF| is the load curve ID defining vent orifice coefficient as a function of relative time. PID LCID Optional part ID of the partition between the interacting control volumes. AREA is based on this part ID. If PID is negative, the blockage of the orifice part due to contact is considered, Load curve ID defining mass flow rate versus pressure difference, see *DEFINE_CURVE. If LCID is defined AREA, SF and PID are ignored. IFLOW Flow direction LT.0: One way flow from AB1 to AB2 only. EQ.0: Two way flow between AB1 and AB2. GT.0: One way flow from AB2 to AB1 only. *AIRBAG_INTERACTION Mass flow rate and temperature load curves for the secondary chambers must be defined as null curves, for example, in the DEFINE_CURVE definitions give two points (0.0, 0.0) and (10000., 0.0). All input options are valid for the following airbag types: *AIRBAG_SIMPLE_AIRBAG_MODEL *AIRBAG_WANG_NEFSKE *AIRBAG_WANG_NEFSKE_JETTING *AIRBAG_WANG_NEFSKE_MULTIPLE_JETTING *AIRBAG_HYBRID *AIRBAG_HYBRID_JETTING The LCID defining mass flow rate vs. pressure difference may additionally be used with: *AIRBAG_LOAD_CURVE *AIRBAG_LINEAR_FLUID If the AREA, SF, and PID defined method is used to define the interaction then the airbags must contain the same gas, i.e. Cp, Cv and g must be the same. The flow between bags is governed by formulae which are similar to those of Wang-Nefske. *AIRBAG_PARTICLE_{OPTION1}_{OPTION2}_{OPTION3}_{OPTION4} Available options include: OPTION1 applies to the MPP implementation only. MPP OPTION2 also applies to the MPP implementation only. When the DECOMPOSITON option is present, LS-DYNA will automatically insert *CONTROL_MPP_DECOMPOSI- TION_BAGREF CONTROL_MPP_DECOMPOSITION_ARRANGE_PARTS keywords if they are not already present in the input. and DECOMPOSITION OPTION3 provides a means to specify an airbag ID number and a heading for the airbag. ID TITLE OPTION4: MOLEFRACTION Purpose: To define an airbag using the particle method. NOTE: This model requires that surface normal vectors be oriented inward, unlike that the traditional CV method for which they must point outward. To check bag and chamber integrity in the CPM model see the CPMERR option on the *CONTROL_CPM card. MPP Card. Additional card for MPP keyword option. 4 5 6 7 8 MPP Variable 1 SX Type F 2 SY F 3 SZ F Default none none none SX, SY, SZ *AIRBAG_PARTICLE DESCRIPTION Scale factor for each direction used during the MPP decomposi- tion. For instance, increasing SX from 1 to 10 will give increase the probability that the model is divided along the 𝑥-direction. Title Card. Additional card for ID or TITLE keyword options. TITLE 1 2 3 4 5 6 7 8 Variable BAGID Type I HEADING A60 The BAGID is referenced in, e.g., *INITIAL_AIRBAG_PARTICLE_POSITION. VARIABLE DESCRIPTION BAGID Airbag ID. This must be a unique number. HEADING Airbag descriptor. It is suggested that unique descriptions be used. Card 1 1 2 3 4 5 6 7 8 Variable SID1 STYPE1 SID2 STYPE2 BLOCK NPDATA FRIC IRPD Type I Default none Card 2 Variable 1 NP I 0 2 I 0 3 I 0 4 I 0 5 I F 0.0 0.0 6 7 I 0 8 UNIT VISFLG TATM PATM NVENT TEND TSW Type I I Default 200,000 0 I 0 F F 293K 1 atm I 0 F F 1010 1010 Optional control card. When the card after Card 2 begins with a “+” character the input reader processes it as this card, otherwise this card is skipped. Card 3 1 2 3 4 5 6 7 8 Variable TSTOP TSMTH OCCUP REBL SIDSV PSID1 Type F F F Default 1010 1msec 0.1 I 0 I I none none Optional unit card. Additional Cards when Unit = 3. Card 4 1 2 3 4 5 6 7 8 Variable Type Mass F Time F Length F Default none none none Card 5 1 2 3 4 5 6 7 8 Variable IAIR NGAS NORIF NID1 NID2 NID3 CHM CD_EXT Type Default I 0 I I none none I 0 I 0 I 0 I F none 0. Internal Part Set Cards. Additional Cards for STYPE2 = 2. Define SID2 cards, one for each internal part or part set. Card 6 1 2 3 4 5 6 7 8 Variable SIDUP STYUP PFRAC LINKING Type I I F I Default none none 0. none Heat Convection Part Set Cards. Additional Cards for NPDATA > 0. Define NPDATA cards, one for each heat convection part or part set. Card 7 1 2 3 4 5 6 7 8 Variable SIDH STYPEH HCONV PFRIC SDFBLK KP INIP Type I I F F F Default none none none none 1.0 F 0. I 0 Vent Hole Card. Additional Cards for NVENT > 0. Define NVENT cards, one for vent hole. Card 8 1 2 3 4 5 6 7 8 Variable SID3 STYPE3 C23 LCTC23 LCPC23 ENH_V PPOP Type Default I 0 I F none 1.0 I 0 I 0 I 0 F 0.0 Air Card. Additional Card for IAIR > 0. Card 9 1 2 3 4 5 6 7 8 Variable PAIR TAIR XMAIR AAIR BAIR CAIR NPAIR NPRLX Type F F F F F F Default PATM TATM none none 0.0 0.0 I 0 I/F 0 MOLEFRACTION Card. Additional card for the MOLEFRACTION option. Card 10 1 2 3 4 5 6 7 8 Variable LCMASS Type I Default none Gas Cards. NGAS additional Cards, one for each gas (card format for ith gas). Card 11 1 2 3 Variable LCMi LCTi XMi Type I I F 4 Ai F 5 Bi F 6 Ci F Default none none none None 0.0 0.0 7 8 INFGi I Orifice Cards. NORIF additional Cards, one for each orifice (card format for ith orifice). Card 12 1 Variable NIDi 2 ANi 3 VDi 4 5 6 7 8 CAi INFOi IMOM IANG CHM_ID Type I F I F Default none none none 30 Deg I 1 I 0 I 0 I 0 VARIABLE DESCRIPTION SID1 Part or part set ID defining the complete airbag. STYPE1 Set type: EQ.0: Part EQ.1: Part set SID2 Part or part set ID defining the internal parts of the airbag. STYPE2 Set type: EQ.0: Part EQ.1: Part set EQ.2: Number of parts to read (Not recommended for general use) VARIABLE DESCRIPTION BLOCK Blocking. Block must be set to a two-digit number BLOCK = M × 10 + N, The 10’s digit controls the treatment of particles that escape due to deleted elements (particles are always tracked and marked). M.EQ.0: Active particle method for which causes particles to be put back into the bag. M.EQ.1: Particles are leaked through vents. See Remark 3. The 1’s digit controls the treatment of leakage. N.EQ.0: Always consider porosity leakage without considering blockage due to contact. N.EQ.1: Check if airbag node is in contact or not. If yes, 1/4 (quad) or 1/3 (tri) of the segment surface will not have porosity leakage due to contact. N.EQ.2: Same as 1 but no blockage for external vents N.EQ.3: Same as 1 but no blockage for internal vents N.EQ.4: Same as 1 but no blockage for all vents. NPDATA Number of parts or part sets data. FRIC IRPD Friction factor. See Remark 2. Dynamic scaling of particle radius. EQ.0: Off EQ.1: On NP Number of particles. (Default = 200,000) UNIT Unit system: EQ.0: kg-mm-ms-K EQ.1: SI EQ.2: tonne-mm-s-K EQ.3: User defined units VISFLG *AIRBAG_PARTICLE DESCRIPTION Visible particles. This field affects only the CPM database. See Remark 5. EQ.0: Default to 1 EQ.1: Output particle's coordinates, velocities, mass, radius, spin energy, translational energy EQ.2: Output reduce data set with coordinates only EQ.3: Suppress CPM database TATM PATM Atmospheric temperature. (Default = 293K) Atmospheric pressure. (Default = 1 ATM) NVENT Number of vent hole parts or part sets TEND TSW Time when all (NP) particles have entered bag. (Default = 1010) Time at which algorithm switches (Default = 1010) to control volumes. TSTOP Time at which front tracking switches from IAIR = 4 to IAIR = 2. TSMTH OCCUP REBL SIDSV To avoid sudden jumps in the pressure signal during switching there is a transition period during which the front tracking is tapered. The default time of 1 millisecond will be applied if this value is set to zero. Particles occupy OCCUP percent of the airbag’s volume. The default value of OCCUP is 10%. This field can be used to balance computational cost and signal quality. OCCUP ranges from 0.001 to 0.1. If the option is ON, all energy stored from damping will be evenly distributed as vibrational energy to all particles. This improves the pressure calculation in certain applications. EQ.0: Off (Default) EQ.1: On Part set ID for internal shell part. The volume occupied by this part is excluded from the bag volume. These internal parts must be consistently orientated for the excluded volume to be correctly calculated. VARIABLE PSID1 DESCRIPTION Part set ID for external parts which have normal pointed outward. This option is usually used with airbag integrity check while there are two CPM bags connected with bag interaction. Therefore, one of the bag can have the correct shell orientation but the share parts for the second bag will have wrong orientation. This option will automatically flip the parts defined in this set in the second bag during integrity checking. Mass, Time, Length Conversion factor from current unit to MKS unit. For example, if the current unit is using kg-mm-ms, the input should be 1.0, 0.001, 0.001 IAIR Initial gas inside bag considered: EQ.0: No EQ.1: Yes, using control volume method. EQ.-1: Yes, using control volume method. In this cake ambient air enters the bag when PATM is greater than bag pres- sure. EQ.2: Yes, using the particle method. EQ.4: Yes, using the particle method. Initial air particles are used for the gas front tracking algorithm but they do not apply forces when they collide with a segment. In- stead, a uniform pressure is applied to the airbag based on the ratio of air and inflator particles. In this case NPRLX must be negative so that forces are not applied by the initial air. NGAS Number of gas components NORIF Number of orifices NID1 - NID3 Three nodes defining a moving coordinate system for the direction of flow through the gas inlet nozzles (Default = fixed system) CHM Chamber ID used in *DEFINE_CPM_CHAMBER. See Remark 7. CD_EXT Drag coefficient for external air. If the value is not zero, the inertial effect from external air will be considered and forces will be applied in the normal direction on the exterior airbag surface. SIDUP *AIRBAG_PARTICLE DESCRIPTION Part or part set ID defining the internal parts that pressure will be applied to. This internal structure acts as a valve to control the external vent hole area. Pressure will be applied only after switch to UP (uniform pressure) using TSW. STYUP Set type: EQ.0: Part EQ.1: Part set PFRAC LINKING Fraction of pressure to be applied to the set (0.0 to 1.0). If PFRAC = 0, no pressure is applied to internal parts. Part ID of an internal part that is coupled to the external vent definition. The minimum area of this part or the vent hole will be used for actual venting area. SIDH Part or part set ID defining part data. STYPEH Set type: EQ.0: Part EQ.1: Part set HCONV Heat convection coefficient used to calculate heat loss from the airbag external surface to ambient (W/K/m2). See *AIRBAG_HY- BRID developments (Resp. P.O. Marklund). LT.0: |HCONV| is a load curve ID defines heat convection coefficient as a function of time. PFRIC Friction factor. PFRIC Defaults to FRIC from 1st card 7th field. SDFBLK Scale down factor for blockage factor (Default = 1, no scale down). The valid factor will be (0,1]. If 0, it will set to 1. KP INIP Thermal conductivity of the part. See Remark 9. Place initial air particles on surface. EQ.0: yes (default) EQ.1: no This feature exclude surfaces from initial particle placement. This option is useful for preventing particles from being trapped between adjacent fabric layers. VARIABLE DESCRIPTION SID3 Part or part set ID defining vent holes. STYPE3 Set type: EQ.0: Part EQ.1: Part set which each part being treated separately EQ.2: Part set and all parts are treated as one vent. See Remark 13. GE..0: Vent hole coefficient, a parameter of Wang-Nefske leakage. A value between 0.0-1.0 can be input, default = 1.0. See Remark 1. LT.0: ID for *DEFINE_CPM_VENT Load curve defining vent hole coefficient as a function of time. LCTC23 can be defined through *DEFINE_CURVE_FUNCTION. If omitted a curve equal to 1 used. See Remark 1. C23 LCTC23 LCPC23 Load curve defining vent hole coefficient as a function of pressure. If omitted a curve equal to 1 is used. See Remark 1. ENH_V Enhanced venting option. See Remark 8. EQ.0: Off (default) EQ.1: On EQ.2: Two way flow for internal vent; treated as hole for external vent Pressure difference between interior and ambient pressure (PATM) to open the vent holes. Once the vents are open, they will stay open. Initial pressure inside bag. (Default PAIR = PATM) Initial temperature inside bag. (Default, TAIR = TATM) PPOP PAIR TAIR XMAIR Molar mass of gas initially inside bag. AAIR - CAIR Constant, linear, and quadratic heat capacity parameters. NPAIR Number of particle for air. See Remark 6. *AIRBAG_PARTICLE DESCRIPTION NPRLX Number of cycles to reach thermal equilibrium. See Remark 6. LT.0: If more than 50% of the collision to fabric is from initial air particle, the contact force will not apply to the fabric segment in order to keep its original shape. If the number contains “.”, “e” or “E”, NPRLX will treated as an end time rather than as a cycle count. LCMASS Total mass flow rate curve for the MOLEFRACTION option. LCMi LCTi XMi Ai - Ci INFGi NIDi ANi VDi flow rate curve Mass the MOLEFRACTION option is used, then it is the time dependent molar fraction of the total flow for gas component i. for gas component i, unless Temperature curve for gas component i. Molar mass of gas component i. Constant, linear, and quadratic heat capacity parameters for gas component i. Inflator ID for this gas component (Defaults to 1). Node ID/Shell ID defining the location of nozzle i. See Remark 12. Area of nozzle i. (Default: all nozzles are assigned the same area) GT.0: Vector ID. Initial direction of gas inflow at nozzle 𝑖. LT.0: Values in the NIDi fields are interpreted as shell IDs. See Remark 12. EQ.-1: direction of gas inflow is using shell normal EQ.-2: direction of gas inflow is in reversed shell normal CAi Cone angle in degrees (Defaults to 30 degrees). This option is used only when IANG equal to 1. INFOi Inflator ID for this orifice. (Default = 1) IMOM Inflator reaction force (R5.1.1 release and later). EQ.0: Off EQ.1: On VARIABLE IANG DESCRIPTION Activation for cone angle to use for friction calibration(not normally used; eliminates thermal energy of particles from inflator). EQ.0: Off (Default) EQ.1: On CHM_ID Chamber ID where the inflator node resides. Chambers are defined using the *DEFINE_CPM_CHAMBER keyword. Remarks: 1. Formula for Total Vent Hole Coefficient. The value must be between 0 and 1. Total vent hole coefficient = min(max(C23 × LCTC23 × LCPC23, 0), 1) 2. Surface Roughtness. Friction factor to simulate the surface roughness. If the surface is frictionless the particle incoming angle 𝛼1is equal to the deflection angle 𝛼2. Considering surface roughness 𝐹r and the total angle 𝛼 will have the following relationships: For the special case when, 0 ≤ 𝐹r ≤ 1 𝛼 = 𝛼1 + 𝛼2 𝐹r = 1 the incoming particle will bounce back from its incoming direction, 𝛼 = 0. For, −1 ≤ 𝐹𝑟 < 0, particles will bounce towards the surface by the following relationship 𝛼 = 2 [𝛼1 − 𝐹𝑟 ( − 𝛼1 )]. 3. Blocking and BLOCK Field. Setting the 10’s digit to 1 allows for physical holes in an airbag. In this case, particles that are far away from the airbag are disabled. In most case, these are particles that have escaped through unclosed surfaces due to physical holes, failed elements, etc. This reduces the bucket sort search distance. 4. Convection Energy Balance. The change in energy due to convection is given by Where, d𝐸 d𝑡 = 𝐴 × HCONV × (𝑇bag − 𝑇atm). 𝐴 = is part area. HCONV = user defined heat convection coefficient. 𝑇bag = the weighted average temperature impacting particles. 𝑇atm = aambient temperature. 5. Output Files. Particle time history data is always output to d3plot database now. LS-PrePost 2.3 and later can display and fringe this data. In order to reduce runtime memory requirements, VISFLG should be set to 0 (disabled). For LS-DYNA 971 R6.1 and later, VISFLG only affects Version 4 CPM output . 6. Spatial Distribution Equilibration for Airbag Particles. Total number of particles used in each card is NP + NPAIR. Since the initial air particles are placed at the surface of the airbag segments with correct velocity distribution initially, particles are not randomly distributed in space. It requires a finite number of relaxation cycles, NPRLX, to allow particles to move and produce better spatial distribution. Since the momentum and energy transfer between particles are based on per- fect elastic collision, CPM solver would like to keep similar mole per particle between inflator and initial air particles. CPM solver will check the following factor. factor = ∣1 − mole per particle of initial air ∣ mole per particle of inflator gas If the factor is more than 10% apart, code will issue the warning message with the tag, (SOL+1232) and provide the suggested NPAIR value. User needs make decision to adjust the NPAIR value based on the application. For example, user setup only initial air without any inflator gas for certain impact analysis should ignore this warning message. 7. Remark Concerning *DEFINE_CPM_CHAMBER. By default initial air particles will be evenly placed on airbag segments which cannot sense the local volume. This will create incorrect pressure field if the bag has several distinct pockets. *DEFINE_CPM_CHAMBER allows the user to initialize air particles by volume ratios of regions of airbag. The particles will be distributed propor- tional to the defined chamber volume to achieve better pressure distribution. 8. Enhanced Venting. When enhanced venting is on, the vent hole’s equivalent radius 𝑅eq will be calculated. Particles within 𝑅eq on the high pressure side from the vent hole geometry center will be moved toward the hole. This will increase the collision frequency near the vent for particles to detect small struc- tural features and produce better flow through the vent hole. ENH_V equals 1, particles are flow from high to low pressure only. EHN_V equals 2, particles can flow in both directions for internal vent. Particles encountering external vents are released. The ambient pressure is not taken into account and the particle will be released regardless the value of the pressure in the bag/chamber. Therefore, the vent rate will be sensitive to the vent location. 9. Effective Convection Heat Transfer Coefficient. If the thermal conductivity, KP, is given, then the effective convection heat transfer coefficient is given by 𝐻eff = ( 1.0 HCONV + shell thickness KP ) −1 , where the part thickness comes from the SECTION database. If KP is not given, 𝐻eff defaults to HCONV. 10. MOLEFRACTION Option. Without the MOLEFRACTION option, a flow rate is specified for each species on the LCMi fields of Card 11. With the MOLE- FRACTION option the total mass flow rate is specified in the LCMASS field on Card 10 and the molar fractions are specified in the LCMi fields of Card 11. 11. User Defined Units. If UNIT = 3 is used, there is no default value for TATM and PATM and user should provide the proper values. User also needs to provide unit conversion factors for code to set correct universal gas constant and some other variables used in the code. 12. Shell Based Nozzle. Node ID and shell ID based nozzle should not be used in the same airbag definition. The nozzle location is taken to be at the center of the shell and the initial nozzle direction can be defined by shell’s normal or by its reversed normal. This vector is transforms with the moving coordinate system defined by NID1 - NID3. The nozzle area is set on the ANi fields and shell area is not taken into account; therefore, the mass flowrate distribution with shells is determined in the same way as it is with nozzles defined by nodes. 13. Merge Part Set for Vent. The first part in the set is designated as the master. All remaining parts are merged into the master so that enhanced venting is treated correctly. ABSTAT_CPM output will be associated with the master part. This option has the same effect as manually merging elements into the master part. *AIRBAG_REFERENCE_GEOMETRY_{OPTION}_{OPTION}_{OPTION} Available options include: <BLANK> BIRTH RDT ID Purpose: If the reference configuration of the airbag is taken as the folded configura- tion, the geometrical accuracy of the deployed bag will be affected by both the stretching and the compression of elements during the folding process. Such element distortions are very difficult to avoid in a folded bag. By reading in a reference configuration such as the final unstretched configuration of a deployed bag, any distortions in the initial geometry of the folded bag will have no effect on the final geometry of the inflated bag. This is because the stresses depend only on the deformation gradient matrix: 𝐹𝑖𝑗 = ∂𝑥𝑖 ∂𝑋𝑗 where the choice of 𝑋𝑗 may coincide with the folded or unfold configurations. It is this unfolded configuration which may be specified here. Note that a reference geometry which is smaller than the initial airbag geometry will not induce initial tensile stresses. If a liner is included and the parameter LNRC set to 1 in *MAT_FABRIC, compression is disabled in the liner until the reference geometry is reached, i.e., the fabric element becomes tensile. When the BIRTH option is specified an additional card setting the BIRTH parameter is activated. The BIRTH parameter specifies a critical time value before which the reference geometry is not used. Until the BIRTH time is reach the input geometry is used for (1) inflating the airbag and for (2) determining the time step size, even when the RDT option is set. NOTE: This card does not support multiple birth times. The last BIRTH value read will be used for all preceding *AIRBAG_REFERENCE_GEOMETRY_BIRTH defini- tions. RGBRTH in *MAT_FABRIC supports a mate- rial dependent birth time. When the RDT option is active the time step size will be based on the reference geometry once the solution time exceeds the birth time. This option is useful for shrunken bags where the bag does not carry compressive loads and the elements can freely expand before stresses develop. If this option is not specified, the time step size will be based on the current configuration and will increase as the area of the elements increase. The default may be much more expensive but possibly more stable. ID card. Additional card for keyword option ID. ID Variable 1 ID Type I 2 SX F 3 SY F 4 SZ F 5 6 7 8 NIDO I Default none 1.0 1.0 1.0 1st NID Birth card. Additional card for keyword option BIRTH. Birth 1 2 3 4 5 6 7 8 Variable BIRTH Type F Default 0.0 Node Cards. For each node ID having an associated reference position include an additional card in format 2. The next “*” keyword card terminates this input. Card 2 1 2 3 4 5 6 7 8 9 10 Variable NID Type I X F Default none 0. Remark Y F 0. Z F 0. VARIABLE DESCRIPTION ID Card ID SX, SY, SZ Scale factor in each direction NIDO Node ID for origin. Default is the first node ID defined in this keyword. BIRTH Time at which the reference geometry activates (default = 0.0) NID X Y Z Node ID for which a reference configuration is defined. Nodes defined in this section must also appear under the *NODE input. It is only necessary to define the reference coordinates of nodal points, if their coordinates are different than those defined in the *NODE section. 𝑥 coordinate 𝑦 coordinate 𝑧 coordinate *AIRBAG_SHELL_REFERENCE_GEOMETRY_{OPTION}_{OPTION} Available options include: <BLANK> RDT ID Purpose: Usually, the input in this section is not needed; however, sometimes it is convenient to use disjoint pre-cut airbag parts to define the reference geometries. If the reference geometry is based only on nodal input, this is not possible since in the assembled airbag the boundary nodes are merged between parts. By including the shell connectivity with the reference geometry, the reference geometry can be based on the pre-cut airbag parts instead of the assembled airbag. The elements, which are defined in this section, must have identical element ID’s as those defined in the *ELEMENT_- SHELL input, but the nodal ID’s, which may be unique, are only used for the reference geometry. These nodes are defined in the *NODE section but can be additionlly defined in *AIRBAG_REFERENCE_GEOMETRY. The element orientation and n1-n4 ordering must be identical to the *ELEMENT_SHELL input. When the RDT option is active the time step size will be based on the reference geometry once the solution time exceeds the birth time which can be defined by RGBRTH of *MAT_FABRIC. ID card. Additional card for keyword option ID. Card 1 Variable 1 ID Type I 2 SX F 3 SY F 4 SZ F 5 NID I Default none 1.0 1.0 1.0 See List 6 7 Card 2 1 2 3 4 5 6 7 8 9 10 Variable EID PID N1 N2 N3 N4 Type I I I I I I Default none none none none none none VARIABLE DESCRIPTION ID Card ID SX, SY, SZ Scale factor in each direction NID EID PID N1 N2 N3 N4 Node ID for origin. Default is the first node ID defined in this keyword. Element ID Optional part ID, see *PART, the part ID is not used in this section. Nodal point 1 Nodal point 2 Nodal point 3 Nodal point 4 ALE does not support implicit time integration nor does it support dynamic relaxation. Furthermore, except for ALE formulation 5, which does support contact, ALE does not, in general, support contact. In three dimensions, ALE supports only one-point solid elements. These solid elements can either be hexahedral, pentahedral, or tetrahedral. Pentahedrons and tetrahedrons are treated as degenerate hexahedron elements. For each ALE multi-material, strain and stress is evaluated in each solid element at a single integration point. In this sense, the ALE element formulation is equivalent to ELEFORM 1 solid formulation. Keywords for the ALE structured solver. *ALE_STRUCTURED_MESH *ALE_STRUCTURED_MESH_CONTROL_POINTS Input required for LS-DYNA’s Arbitrary-Lagrangian-Eulerian capability is defined using *ALE cards. The keyword cards in this section are defined in alphabetical order: *ALE_AMBIENT_HYDROSTATIC *ALE_COUPLING_NODAL_CONSTRAINT *ALE_COUPLING_NODAL_DRAG *ALE_COUPLING_NODAL_PENALTY *ALE_COUPLING_RIGID_BODY *ALE_ESSENTIAL_BOUNDARY *ALE_FAIL_SWITCH_MMG *ALE_FRAGMENTATION *ALE_FSI_PROJECTION *ALE_FSI_SWITCH_MMG_{OPTION} *ALE_FSI_TO_LOAD_NODE *ALE_MULTI-MATERIAL_GROUP *ALE_REFERENCE_SYSTEM_CURVE *ALE_REFERENCE_SYSTEM_NODE *ALE_REFERENCE_SYSTEM_SWITCH *ALE_REFINE *ALE_SMOOTHING *ALE_TANK_TEST *ALE_UP_SWITCH For other input information related to the ALE capability, see keywords: *ALE_TANK_TEST *BOUNDARY_AMBIENT_EOS *CONSTRAINED_EULER_IN_EULER *CONSTRAINED_LAGRANGE_IN_SOLID *CONTROL_ALE *DATABASE_FSI *INITIAL_VOID *INITIAL_VOLUME_FRACTION *INITIAL_VOLUME_FRACTION_GEOMETRY *SECTION_SOLID *SECTION_POINT_SOURCE_FOR_GAS_ONLY *SECTION_POINT_SOURCE_MIXTURE *SET_MULTIMATERIAL_GROUP_LIST *CONSTRAINED_EULER_IN_EULER For a single gaseous material: *EOS_LINEAR_POLYNOMIAL *EOS_IDEAL_GAS For multiple gaseous materials: *MAT_GAS_MIXTURE *INTIAL_GAS_MIXTURE *ALE_AMBIENT_HYDROSTATIC Purpose: When an ALE model contains one or more ambient (or reservoir-type) ALE parts (ELFORM = 11 and AET = 4), this command may be used to initialize the hydrostatic pressure field in the ambient ALE domain due to gravity. The *LOAD_- BODY_{OPTION} keyword must be defined. The associated *INITIAL_HYDROSTAT- IC_ALE keyword may be used to define a similar initial hydrostatic pressure field for the regular ALE domain (not reservoir-type region). Card 1 1 2 3 4 5 6 7 8 Variable ALESID STYPE VECID GRAV PBASE RAMPTLC Type I Default none Card 2 1 I 0 2 I none 3 I 0 4 I 0 5 I 0 6 7 8 Variable NID MMGBL Type I I Default None none VARIABLE ALESID DESCRIPTION ALESID defines the reservoir-type ALE domain/mesh whose hydrostatic pressure field due to gravity is being initialized by this keyword. See Remark 4. STYPE ALESID set type. See Remark 4. EQ.0: Part set ID (PSID), EQ.1: Part ID (PID) ), EQ.2: Solid set ID (SSID). VECID Vector ID of a vector defining the direction of gravity. VARIABLE DESCRIPTION GRAV PBASE Magnitude of the Gravitational acceleration. For example, in metric units the value is usually set to 9.80665 m/s2. Nominal or reference pressure at the top surface of all fluid layers. By convention, the gravity direction points from the top layer to the bottom layer. Each fluid layer must be represented by an ALE multi-material group ID (AMMGID or MMG). See Remark 1. RAMPTLC A ramping time function load curve ID. This curve (via *DE- FINE_CURVE) defines how gravity is ramped up as a function of time. Given GRAV value above, the curve’s ordinate varies from 0.0 to 1.0, and its abscissa is the (ramping) time. See Remark 2. NID Node ID defining the top of an ALE fluid (AMMG) layer. MMGBL AMMG ID of the fluid layer immediately below this NID. Each node is defined in association with one AMMG layer below it. See Remark 4. Remarks: 1. Pressure in Multi-Layer Fluids. For models using multi-layer ALE Fluids the pressure at the top surface of the top fluid layer is set to PBASE and the hydro- static pressure is computed as following 𝑁layers 𝑃 = 𝑃base + ∑ 𝜌𝑖𝑔ℎ𝑖 . 𝑖=1 2. Hydrostatic Pressure Ramp Up. If RAMPTLC is activated (i.e. not equal to “0”), then the hydrostatic pressure is effectively ramped up over a user-defined duration and kept steady. When this load curve is defined, do not define the associated *INITIAL_HYDROSTATIC_ALE card to initialize the hydrostatic pressure for the non-reservoir ALE domain. The hydrostatic pressure in the regular ALE region will be initialized indirectly as a consequence of the hydro- static pressure generated in the reservoir-type ALE domain. The same load curve should be used to ramp up gravity in a corresponding *LOAD_- BODY_(OPTION) card. Via this approach, any submerged Lagrangian struc- ture coupled to the ALE fluids will have time to equilibrate to the proper hydrostatic condition. 3. Limitation on EOS Model. The keyword only supports *EOS_GRUNEISEN and *EOS_LINEAR_POLYNOMIAL, but only inthe following two cases, 𝑐4 = 𝑐5 > 0, 𝑐3 = 𝑐4 = 𝑐5 = 𝑐6 = 0, 𝑐1 = 𝑐2 = 𝑐3 = 𝑐6 = 0, 𝐸0 = 0 𝑉0 = 0. 4. Structured ALE usage. When used with structured ALE, PART and PART set options might not make too much sense. This is because all elements inside a structured ALE mesh are assigned to one single PART ID. In the Structured ALE case, we should generate a solid set which contains those ALE boundary elements we want to prescribe hydrostatic pressures on. It is done by using the *SET_SOLID_GENERAL keyword with SALECPT option. And then use the STYPE=2 option (Solid element set ID). Example: Model Summary: Consider a model consisting of 2 ALE parts, air on top of water. H3 = AMMG1 = Air part above H4 = AMMG2 = Water part below $...|....1....|....2....|....3....|....4....|....5....|....6....|....7....|....8 $ ALE materials (fluids) listed from top to bottom: $ $ NID AT TOP OF A LAYER SURFACE ALE MATERIAL LAYER BELOW THIS NODE $ TOP OF 1st LAYER -------> 1681 ---------------------------------------- $ Air above = PID 3 = H3 = AMMG1 (AET=4) $ TOP OF 2nd LAYER -------> 1671 ---------------------------------------- $ Water below = PID 4 = H4 = AMMG2 (AET=4) $ BOTTOM --------------------> ---------------------------------------- $...|....1....|....2....|....3....|....4....|....5....|....6....|....7....|....8 *ALE_AMBIENT_HYDROSTATIC $ ALESID STYPE VECID GRAV PBASE RAMPTLC 34 0 11 9.80665 101325.0 9 $ NID MMGBL 1681 1 1671 2 *SET_PART_LIST 34 3 4 *ALE_MULTI-MATERIAL_GROUP 3 1 4 1 *DEFINE_VECTOR $ VID XT YT ZT XH YH ZH CID 11 0.0 1.0 0.0 0.0 0.0 0.0 *DEFINE_CURVE 9 0.000 0.000 0.001 1.000 10.000 1.000 *LOAD_BODY_Y $ LCID SF LCIDDR XC YC ZC 9 9.80665 0 0.0 0.0 0.0 $...|....1....|....2....|....3....|....4....|....5....|....6....|....7....|....8 *ALE_COUPLING_NODAL_CONSTRAINT_{OPTION} Available options include: <BLANK> ID TITLE Purpose: This keyword activates constraint coupling between ALE materials (master) and non-ALE nodes. The slave nodes may belong to Lagrangian solid, shell, beam, thick shell, or discrete sphere elements. In contrast to *ALE_COUPLING_NODAL_PENALTY, caution should be exercised in connection with EFG and SPH nodes, as meshless methods generally do not satisfy essential boundary conditions, leading to energy dissipation. This keyword requires a 3D ALE formulation. It is, there- fore, incompatible with parts defined using *SECTION_- ALE2D or *SECTION_ALE1D. If a title is not defined LS-DYNA will automatically create an internal title for this coupling definition. Title Card. Additional card for TITLE and ID keyword options. Title 1 2 3 4 5 6 7 8 Variable COUPID Type I TITLE A70 Card 1 1 2 3 4 5 6 7 8 Variable SLAVE MASTER SSTYP MSTYP CTYPE MCOUP Type I I Default none none I 0 I 0 I 1 I Card 2 1 2 3 4 5 6 7 8 Variable START END Type Default F 0 F 1.0E10 FRCMIN F 0.5 VARIABLE COUPID DESCRIPTION Coupling (card) ID number (I10). If not defined, LSDYNA will assign an internal coupling ID based on the order of appearance in the input deck. TITLE A description of this coupling definition (A70). SLAVE Slave set ID defining a part, part set or segment set ID of the Lagrangian or slave structure . See Remark 1. MASTER Master set ID defining a part or part set ID of the ALE or master solid elements . SSTYP Slave set type of “SLAVE”: EQ.0: part set ID (PSID). EQ.1: part ID (PID). EQ.2: segment set ID (SGSID). EQ.3: node set ID (NSID). MSTYP Master set type of “MASTER”: EQ.0: part set ID (PSID). EQ.1: part ID (PID). CTYPE Coupling type: EQ.1: constrained velocity only. EQ.2: constrained acceleration and velocity. MCOUP Multi-material option . EQ.0: couple with all multi-material groups, VARIABLE DESCRIPTION LT.0: MCOUP must be an integer. –MCOUP refers to a set ID of an ALE multi-material groups defined in *SET_MUL- TI-MATERIAL_GROUP. START Start time for coupling. END End time for coupling. FRCMIN Only to be used with nonzero MCOUP. Minimum volume fraction of the fluid materials included in the list of AMMGs to activate coupling. Default value is 0.5. Remarks: When MCOUP is a negative integer, say for example MCOUP = -123, then an ALE multi-material set-ID (AMMSID) of 123 must exist. This is an ID defined by a *SET_- MULTI-MATERIAL_GROUP_LIST card. *ALE_COUPLING_NODAL_DRAG Available options include: <BLANK> ID TITLE Purpose: This command provides a coupling mechanism to model the drag interaction between ALE fluids, which provide the master elements, and discrete element forms, which comprise the slave nodes. The slave nodes are assumed to be of spherical shape being either SPH elements, or discrete elements (*ELEMENT_DISCRETE_SPHERE). The coupling forces are proportional to the relative speed between the fluid and particles plus the buoyancy force due to gravitational loading. This keyword requires a 3D ALE formulation. It is, there- fore, incompatible with parts defined using *SECTION_- ALE2D or *SECTION_ALE1D. If a title is not defined, LS-DYNA will automatically generate an internal title for this coupling definition. Title Card. Additional card for TITLE and ID keyword options. Title 1 2 3 4 5 6 7 8 Variable COUPID Type I TITLE A70 Card 1 1 2 3 4 5 6 7 8 Variable SLAVE MASTER SSTYP MSTYP Type I I Default none none I 0 I Card 2 1 2 3 4 5 6 7 8 Variable START END FCOEF DIRECG GRAV Type Default F 0 F 1.0E10 F 1.0 I F none 0.0 VARIABLE COUPID DESCRIPTION Coupling (card) ID number (I10). If not defined, LSDYNA will assign an internal coupling ID based on the order of appearance in the input deck. TITLE A description of this coupling definition (A70). SLAVE Slave set ID defining a part, part set or segment set ID of the Lagrangian or slave structure . MASTER Master set ID defining a part or part set ID of the ALE or master solid elements . SSTYP Slave set type of “SLAVE”: EQ.0: part set ID (PSID). EQ.1: part ID (PID). EQ.2: segment set ID (SGSID). EQ.3: node set ID (NSID). MSTYP Master set type of “MASTER”: EQ.0: part set ID (PSID). EQ.1: part ID (PID). START Start time for coupling. END End time for coupling. FCOEF *ALE_COUPLING_NODAL_DRAG DESCRIPTION Drag coefficient scale factor or function ID to calculate drag coefficient GT.0: Drag coefficient scale factor. LT.0: The absolute value of FCOEF is the Function ID of the user provided function to calculate drag coefficient; See Remark 1. DIRECG Gravity force direction. EQ.1: Global x direction EQ.2: Global y direction EQ.3: Global z direction GRAV Gravity value. This value is used to calculate buoyance force. Remarks: 1. Drag Coupling Force. The drag coupling force in between the particles and ALE fluids takes the following form. 𝐹drag = 𝑐drag × 1 𝜌𝑣2 × 1 𝜋𝑑2 where 𝑐drag is the drag coefficient, 𝜌 the fluid density in which the particle is submerged, 𝑣 the relative velocity between the particle and the fluid, 𝑑 the diameter of the particle. The default drag coefficient is a function of Reynolds’s number and calculated by using the following formula: 𝑐drag = ⎜⎛0.63 + ⎝ . 4.8 ⎟⎞ √Re⎠ Users can define their own function of drag coefficient. To do that, one needs to define a function using *DEFINE_FUNCTION and assign the negative function ID to FCOEF flag. An example is provided below to illustrate the setup. It is equivalent to the default drag coefficient calculation. *ALE_COUPLING_NODAL_DRAG 10001 1 3 1 -10 3 9.81 *DEFINE_FUNCTION 10 float cd(float re) { float cd; cd=(0.63+4.8/sqrt(re))*(0.63+4.8/sqrt(re)); if (cd > 2.0) cd = 2.0; return cd; } *ALE_COUPLING_NODAL_PENALTY Available options include: <BLANK> ID TITLE Purpose: This command provides a penalty coupling mechanism between ALE materials (master) and non-ALE nodes (slave). The slave nodes may belong to Lagrangian solid, shell, beam, thick shell, or discrete (*ELEMENT_DISCRETE_SPHERE) elements. In contrast to *ALE_COUPLING_NODAL_CONSTRAINT, SPH and EFG nodes are supported. This keyword is incompatible with parts that use *SEC- TION_ALE2D or *SECTION_ALE1D, i.e., it requires a 3D ALE formulation. If a title is not defined LS-DYNA will automatically create an internal title for this coupling definition. Title Card. Additional card for TITLE and ID keyword options. Title 1 2 3 4 5 6 7 8 Variable COUPID Type I TITLE A70 Card 1 1 2 3 4 5 6 7 8 Variable SLAVE MASTER SSTYP MSTYP MCOUP Type I I Default none none I 0 I 0 I Card 2 1 2 3 4 5 6 7 8 Variable START END PFORM PFAC FRCMIN Type Default F 0 F 1.0E10 I 0 F 0.1 F 0.5 VARIABLE COUPID DESCRIPTION Coupling (card) ID number (I10). If not defined, LSDYNA will assign an internal coupling ID based on the order of appearance in the input deck. TITLE A description of this coupling definition (A70). SLAVE Slave set ID defining a part, part set or segment set ID of the Lagrangian or slave structure . See Remark 1. MASTER Master set ID defining a part or part set ID of the ALE or master solid elements . SSTYP Slave set type of “SLAVE”: EQ.0: part set ID (PSID). EQ.1: part ID (PID). EQ.2: segment set ID (SGSID). EQ.3: node set ID (NSID). MSTYP Master set type of “MASTER”: EQ.0: part set ID (PSID). EQ.1: part ID (PID). MCOUP Multi-material option . EQ.0: couple with all multi-material groups, LT.0: MCOUP must be an integer. –MCOUP refers to a set ID of an ALE multi-material groups defined in *SET_MUL- TI-MATERIAL_GROUP. START Start time for coupling. VARIABLE DESCRIPTION END End time for coupling. PFORM Penalty stiffness formulations. EQ.0: mass based penalty stiffness. EQ.1: bulk modulus based penalty stiffness. EQ.2: penalty stiffness is determined by the user-provided load curve between penetration and penalty pressure. Penalty stiffness factor (PFORM = 0 or 1) for scaling the estimated stiffness of the interacting (coupling) system or Load Curve ID (PFORM = 2). Only to be used with nonzero MCOUP. Minimum volume fraction of the fluid materials included in the list of AMMGs to activate coupling. Default value is 0.5. PFAC FRCMIN Remarks: When MCOUP is a negative integer, say for example MCOUP = -123, then an ALE multi-material set-ID (AMMSID) of 123 must exist. This is an ID defined by a *SET_- MULTI-MATERIAL_GROUP_LIST card. *ALE Purpose: This command serves as a simplified constraint type coupling method between ALE fluids and a Lagrange rigid body. In certain FSI simulations structure deformation is either small or not of the interest. Often times these structures are modeled as rigid bodies to shorten the simulation time and reduce the complexity. For such kind of problems, a full scale ALE/FSI simulation is costly in both simulation time and memory. This keyword provides a light-weight alternative FSI method for systems with minimal structural response. It has a similar input format to *ALE_ESSENTIAL_BOUNDARY and maybe regarded as being an extension of the essential boundary feature. The documentation for *ALE_- ESSENTIAL_BOUNDARY_BODY applies, in large part, to this card also. Card 1 1 2 3 4 5 6 7 8 Variable IPID NSID Type I I Default none none ALE Coupling Interfaces Cards. Include one card for each part, part set or segment to define ALE coupling interface. This input ends at the next keyword (“*”) card. Card 2 Variable 1 ID 2 3 4 5 6 7 8 IDTYPE ICTYPE IEXCL Type I I Default none none I 1 I none VARIABLE DESCRIPTION IPID NSID Rigid body part ID. Node set ID defining ALE boundary nodes to follow Rigid body motion. VARIABLE DESCRIPTION ID Set ID defining a part, part set or segment set ID of the ALE coupling interface. IDTYPE Type of set ID: EQ.0: part set ID (PSID). EQ.1: part ID (PID). EQ.2: segment set ID (SGSID). ICTYPE Constraint type: EQ.1: No flow through all directions. EQ.2: No flow through normal direction. (slip condition) IEXCL Segment Set ID to be excluded from applying ALE essential boundary condition. For example, inlet/outlet segments. Remarks: For ICTYPE = 2, the constrained direction(s) at each surface node comes in part from knowing whether the node is a surface node, an edge node, or a corner node. If the ALE mesh boundary is identified by part(s) (IDTYPE = 0/1), edge and corner nodes are automatically detected during the segment generation process. However, this automatic detection is not foolproof for complicated geometries. Identifying the ALE mesh boundary using segment sets (IDTYPE = 2) is generally preferred for complicated geometries in order to avoid misidentification of edge and corner nodes. When segment sets are used, the edge and corner nodes are identified by their presence in multiple segment sets where each segment set describes a more or less smooth, continuous surface. The intersections of these surfaces are used to identify edge/corner nodes. *ALE Purpose: This command applies and updates essential boundary conditions on ALE boundary surface nodes. Updating the boundary conditions is important if the ALE mesh moves according to *ALE_REFERENCE_SYSTEM_GROUP. If the mesh does not move, it’s more correct to call it an Eulerian mesh rather than an ALE mesh, but *ALE_- ESSENTIAL_BOUNDARY can be applied nonetheless. Certain engineering problems need to constrain the flow along the ALE mesh boundary. A simple example would be water flowing in a curved tube. Using the *ALE_ESSENTIAL_BOUNDARY approach, the tube material is not modeled and there is no force coupling between the fluid and the tube, rather the interior volume of the tube is represented by the location of the ALE mesh. Defining SPC boundary conditions with a local coordinate system at each ALE boundary node would be extremely inconvenient in such a situation. The *ALE_ESSENTIAL_BOUNDARY command applies the desired constraints along the ALE surface mesh automatically. The user only needs to specify the part(s) or segment set(s) corresponding to the ALE boundary surfaces and the type of constraint desired. Boundary Condition Cards. Include one card for each part, part set or segment on which essential boundary conditions are applied. This input ends at the next keyword (“*”) card. Card 1 Variable 1 ID 2 3 4 5 6 7 8 IDTYPE ICTYPE IEXCL Type I I Default none none I 1 I none VARIABLE DESCRIPTION ID Set ID defining a part, part set or segment set ID of the ALE mesh boundary. IDTYPE Type of set ID: EQ.0: part set ID (PSID). EQ.1: part ID (PID). EQ.2: segment set ID (SGSID). VARIABLE DESCRIPTION ICTYPE Constraint type: EQ.1: No flow through all directions. EQ.2: No flow through normal direction. (slip condition) IEXCL Segment Set ID to be excluded from applying ALE essential boundary condition. For example, inlet/outlet segments. Remarks: For ICTYPE = 2, the constrained direction(s) at each surface node comes in part from knowing whether the node is a surface node, an edge node, or a corner node. If the ALE mesh boundary is identified by part(s) (IDTYPE = 0/1), edge/corner nodes are automatically detected during the segment generation process. However, this automatic detection is not foolproof for complicated geometries. Identifying the ALE mesh boundary using segment sets (IDTYPE = 2) is generally preferred for complicated geometries in order to avoid misidentification of edge/corner nodes. When segment sets are used, the edge/corner nodes are identified by their presence in multiple segment sets where each segment set describes a more or less smooth, continuous surface. In short, the junctures or intersections of these surfaces identify edge/corner nodes. *ALE Purpose: This card is used to allow the switching of an ALE multi-material-group ID (AMMGID) if a failure criteria is reached. If this card is not used and *MAT_VACUUM has a multi-material group in the input deck, failed ALE groups are replaced by the group for *MAT_VACUUM. Available options include: <BLANK> ID TITLE A title for the card may be input between the 11th and 80th character on the title-ID line. The optional title line precedes all other cards for this command. The user can explicitly define a title for this coupling. Title Card. Additional card for the ID or TITLE options to keyword. Title Variable 1 ID Type I10 2 3 4 5 6 7 8 TITLE A70 Card 1 1 2 3 4 5 6 7 8 Variable FR_MMG TO_MMG Type I I Default none none VARIABLE FR_MMG DESCRIPTION This is the AMMG-SID before the switch. The AMMG-SID corresponds to the SID defined under the *SET_MULTI-MATERI- AL_GROUP_LIST (SMMGL) card. This SID points to one or more AMMGs. See Remark 1. This is the AMMG-SID after the switch. The AMMG-SID corresponds to the SID defined under the *SET_MULTI-MATERI- AL_GROUP_LIST card. This SID points to one or more AMMGs. See Remark 1. *ALE VARIABLE TO_MMG Remarks: 1. There is a correspondence between the FR_MMG and TO_MMG. Consider an example where: a) The FR_MMG SID points to a SID = 12 (the SID of its SMMGL card is 12, and this SID contains AMMG 1 and AMMG 2) b) The TO_MMG points to a SID = 34 (the SID of the SMMGL card is 34, and this SID contains AMMG 3 and AMMG 4) Then, AMMG 1, if switched, will become AMMG 3, and AMMG 2, if switched, will become AMMG 4. *ALE Purpose: When a material fails, this card is used to switch the failed material to When used with FRAGTYP = 2, it can be used to model material vacuum. fragmentation. Card 1 1 2 3 4 5 6 7 8 Variable FR_MMG TO_MMG FRAGTYP Type I I I Default none none none DESCRIPTION This is the AMMGID of the material that just fails, before the switch. This is the AMMGID of the vacuum that the failed material is being switched to. Flag defining whether the failed material is completely or partially switched to vacuum . EQ.1: Fully switch; all failed material is switched to vacuum. EQ.2: Partially switch; only the volume expansion from the last time step is switched to vacuum. VARIABLE FR_MMG TO_MMG FRAGTYP Remarks: The Lagrange element contains only one material. Once the failure criterion is met in a Lagrange element, the whole element is marked as “failed” and either deleted or kept from further element force calculation. However, for multi-material ALE elements, such approach is not practical as these elements are occupied by multiple materials. Failure, therefore, cannot be adequately modeled at the element level. Instead we convert the failed material inside an ALE element to vacuum. The effect is similar to element deletion in Lagrange simulations. The failed material, once switched to vacuum, is excluded from any future element force calculation. 1. Switch to Vacuum, (FRAGTYPE = 1). By default multi-material elements switch failed materials to vacuum. This switch involves assigning the full vol- ume fraction of the failed material, say AMMG 1, in an element to vacuum, say AMMG 2. FRAGTYP = 1 is equivalent to the default treatment. However, with this card the vacuum AMMG can be explicitly specified. In the case that more than one vacuum AMMG exist, it is strongly recommended to use the FRAGTYP = 1 approach to eliminate ambiguity. It is also helpful during post-processing since it is possible to see the material interface of the switched material by assigning a dedicated vacuum AMMG to the switched material. 2. Fragmentation, (FRAGTYPE = 2). FRAGYP = 2 models material fragmenta- tion. Note that the FRAGTYP = 1 approach leads to loss of mass and, conse- quently, dissipates both momentum and energy. With FRAGTYP = 2, instead of converting the full volume of the failed material to vacuum, LS-DYNA only converts the material expansion to vacuum. This approach conserves mass and, therefore, momentum and energy. To illustrate how this fragmentation model works, consider a tension failure example. At the time step when the material fails, LS-DYNA calculates the material expansion in the current step and converts this volume to vacuum. The stresses and other history variables are left unchanged, so that in the next time step it will again fail. The expansion in the next time step will be also converted to vacuum. This process continues until maybe at a later time the gap stops growing or even starts to close due to compression. Example: Consider a simple bar extension example: FR_MMG: H5 = AMMG1 = Metal bar H6 = AMMG2 = Ambient air TO_MMG: H7 = AMMG3 = Dummy vacuum part $...|....1....|....2....|....3....|....4....|....5....|....6....|....7....|....8 *ALE_FRAGMENTATION $ FR_MMG TO_MMG FRAGTYP 1 3 2 $...|....1....|....2....|....3....|....4....|....5....|....6....|....7....|....8 *ALE Purpose: This card provides a coupling method for simulating the interaction between a Lagrangian material set (structure) and ALE material set (fluid). The nearest ALE nodes are projected onto the Lagrangian structure surface at each time step. This method does not conserve energy, as mass and momentum are transferred via constrained based approach. Card 1 1 2 3 4 5 6 7 8 Variable LAGSID ALESID LSIDTYP ASIDTYP SMMGID ICORREC INORM I 0 3 I 0 4 I 0 5 I 0 6 I 0 7 8 Type Default I 0 Card 2 1 I 0 2 Variable BIRTH DEATH Type F F Default 0.0 1.E+10 VARIABLE LAGSID DESCRIPTION A set ID defining the Lagrangian part(s) for this coupling (structures). ALESID A set ID defining the ALE part(s) for this coupling (fluids). LSIDTYP Lagrangian set ID type EQ.0: Part set ID (PSID), EQ.1: Part ID (PID). ASIDTYP ALE set ID type EQ.0: Part set ID (PSID), EQ.1: Part ID (PID). SMMGID *ALE_FSI_PROJECTION DESCRIPTION A set ID referring to a group of one or more ALE-Multi-Material- Group (AMMG) IDs which represents the ALE materials interacting with the Lagrangian structure. This SMMGID is a set ID defined by *SET_MULTI-MATERIAL_GROUP_LIST. ICORREC Advection error correction method . EQ.1: ALE mass is conserved. Leaked mass is moved, EQ.2: ALE mass is almost conserved, EQ.3: No correction performed (default). is conserved. Some leakage may occur. This may be the best solution. ALE mass INORM Type of coupling. EQ.0: Couple in all directions, EQ.1: Couple in compression and tension (free sliding), EQ.2: Couple in compression only (free sliding). This choice requires ICORREC = 3. BIRTH Start time for coupling. DEATH End time for coupling. Remarks: 1. As the ALE nodes are projected onto the closest Lagrangian surface, there may be some advection errors introduced. These errors may result in a small ele- ment mass fraction being present on the “wrong” side of the coupled Lagrangi- an surface. There are 3 possible scenarios: a) Mass on the wrong side of the Lagrangian structure may be moved to the right side. This may cause P oscillations. No leakage will occur. b) Mass on the wrong side is deleted. Mass on the right side is scaled up to compensate for the lost mass. No leakage will occur. c) Mass on the wrong side is allowed (no correction performed). Some leak- age may occur. This may be the most robust and simplest approach. Model Summary: *ALE H1 = AMMG1 = background air mesh H2 = AMMG1 = background air mesh S3 = cylinder containing AMMG2 S4 = dummy target cylinder for impact The gas inside S3 is AMMG2. S3 is given an initial velocity and it will impact S4. $...|....1....|....2....|....3....|....4....|....5....|....6....|....7....|....8 *ALE_MULTI-MATERIAL_GROUP 1 1 2 1 *SET_MULTI-MATERIAL_GROUP_LIST 22 2 *ALE_FSI_PROJECTION $ LAGSID ALESID LSIDTYP ASIDTYP SMMGID ICORREC INORM 3 1 1 1 22 3 2 $ BIRTH DEATH 0.0 20.0 $...|....1....|....2....|....3....|....4....|....5....|....6....|....7....|....8 *ALE_FSI_SWITCH_MMG Purpose: This card is used to allow the switching of an ALE multi-material-group ID (AMMGID) of a fluid as that fluid passes across a monitoring surface. This monitoring surface may be a Lagrangian shell structure, or a segment set. It does not have to be included in the slave set of the coupling card: *CONSTRAINED_LAGRANGE_IN_SOL- ID. However, at least one coupling card must be present in the model. Available options include: <BLANK> ID TITLE An ID number (up to 8 digits) may be defined for this switch command in the first 10- character space. A title for the card may be input between the 11th and 80th character on the title-ID line. The optional title line precedes all other cards for this command. The user can explicitly define a title for this coupling. Title Card. Additional card for the Title or ID keyword options. Title Variable 1 ID Type I10 2 3 4 5 6 7 8 TITLE A70 Card 1 1 2 3 4 5 6 7 8 Variable SID STYPE NQUAD XOFF BTIME DTIME NFREQ NFOLD Type I Default none I 0 I 1 F F F 0.0 0.0 1.0E20 I 1 I Card 2 1 2 3 4 5 6 7 8 Variable FR_MMG TO_MMG XLEN Type I I F Default none none 0.0 VARIABLE SID DESCRIPTION A set ID defining a monitoring surface over which an ALE fluid flows across, and its ALE multi-material-group-ID (AMMGID) is switched. The monitoring surface may be a Lagrangian shell structure, or a segment set. This surface, if Lagrangian, does not have to be included in the coupling definition . STYPE Set ID type of the above SID. EQ.0: Part set ID (PSID) (default). EQ.1: Part ID (PID). EQ.2: Segment set ID (SGSID). NQUAD XOFF The number of flow-sensor points to be distributed over each monitoring surface/segment. There should be enough sensor points distributed to monitor the flow in each ALE element intersected by this monitoring surface (default = 1, see remark 3). An offset distance away from the monitoring surface, beyond which the AMMGID switching occurs. The direction of XOFF is defined by the normal vector of the monitoring segment. This offset distance, in general, should be at least 2 ALE element widths away from, and beyond the monitoring interface (default = 0.0). BTIME Start time for the AMMGID switch to be activated (default = 0.0). DTIME Ending time for the AMMGID switch (default = 1.0E20). NFREQ Number of computational cycles between ALE switch check (default = 1). Flag for checking folding logic (default = 0, ⇒ off). If NFOLD = 1 (⇒ on), then LS-DYNA will check if the monitoring segment is in the fold, applicable to airbag. If the monitoring segment is still located within a folded (shell) region, then no switching is allowed yet until it has unfolded. This is the AMMG-SID before the switch. The AMMG-SID corresponds to the SID defined under the *SET_MULTI-MATERI- AL_GROUP_LIST (SMMGL) card. This SID points to one or more AMMGs. See Remark 1. This is the AMMG-SID after the switch. The AMMG-SID corresponds to the SID defined under the *SET_MULTI-MATERI- AL_GROUP_LIST card. This SID points to one or more AMMGs. See Remark 1. This is an absolute distance for distributing the flow sensor points over the ALE elements. To make sure that at least 1 sensor point, defined on each Lagrangian segment, is present in each ALE element to track the flow of an AMMG, XLEN may be estimated as roughly half the length of the smallest ALE element in the mesh. See Remark 3. *ALE VARIABLE NFOLD FR_MMG TO_MMG XLEN Remarks: 1. There is a correspondence between the FR_MMG and TO_MMG. Consider an example where: a) The FR_MMG SID points to a SID = 12 (the SID of its SMMGL card is 12, and this SID contains AMMG 1 and AMMG 2) b) The TO_MMG points to a SID = 34 (the SID of the SMMGL card is 34, and this SID contains AMMG 3 and AMMG 4) Then, AMMG 1, if switched, will become AMMG 3, and AMMG 2, if switched, will become AMMG 4. 2. The ID option must be activated if the parameter SWID is used in the *DATA- BAS_FSI card. Then the accumulated mass of an AMMG that goes through a tracking surface, and being switched, will be reported via the parameter “mout” in the “dbfsi” ASCII output file (or equivalently the “POROSITY” pa- rameter inside LS-PrePost ASCII plotting option). 3. When both NQUAD and XLEN are defined, whichever gives smaller sensor- point interval distance will be used. XLEN may give better control as in the case of a null shell acting as the monitoring surface. As this null shell is stretched, NQUAD distribution of sensor-points may not be adequate, but XLEN would be. 4. The monitoring surface does not have to be included in the slave set of the coupling card. However, at least one coupling card must be present in the model. The monitoring segment set can be made up of Lagrangian or ALE nodes. Example: Consider a simple airbag model with 3 part IDs: H25 (AMMG1) = Inflator gas injected into the airbag. H24 (AMMG2) = Air outside the airbag (background mesh). H26 (AMMG3) = Dummy AMMG of inflator gas after it passes through a vent hole. S9 = A Lagrangian shell part representing a vent hole. S1 = A Lagrangian shell part representing the top half of an airbag. S2 = A Lagrangian shell part representing the bottom half of an airbag. The inflator gas inside the airbag is distinguished from the inflator gas that has passed through the monitoring surface (vent hole) to the outside of the airbag by assigning different ALE multi-material group set ID to each. The dummy fluid part (H26) should have the same material and EOS model IDs as the before-switched fluid (H25). TO_MMG = 125 ⇒ AMMGID (before switch) = *SET_MULTI-MATERIAL_GROUP_LIST(125) = 1 ⇒ PART = PART(AMMGID1) = H25 FR_MMG = 126 ⇒ AMMGID (before switch) = *SET_MULTI-MATERIAL_GROUP_LIST(126) = 3 ⇒ PART = PART(AMMGID3) = H26 $...|....1....|....2....|....3....|....4....|....5....|....6....|....7....|....8 *ALE_MULTI-MATERIAL_GROUP 25 1 24 1 26 1 *DATABASE_FSI $ TOUT [STYPE: 0=PSID ; 1=PID ; 2=SGSID] 0.1000 $ DBFSI_ID SID STYPE AMMGSWID LDCONVID 1 1 1 2 2 1 3 9 1 90000 *SET_MULTI-MATERIAL_GROUP_LIST 125 1 *SET_MULTI-MATERIAL_GROUP_LIST 126 3 *ALE_FSI_SWITCH_MMG_ID 90000 $ SID SIDTYPE NQUAD XOFF BTIME DTIME NFREQ FOLD 9 1 3 -20.0 5.0 0.0 1 1 $ Fr_MMG To_MMG XCLEN 125 126 5. $...|....1....|....2....|....3....|....4....|....5....|....6....|....7....|....8 Note: 1. The *DATABASE_FSI card tracks 3 surface entities: (a) top half of an airbag, (b) bottom half of an airbag, and (c) the vent hole monitoring surface where the AMMGID of the inflator gas is switched. 2. The amount of mass passing through the vent hole during the switch is output to a parameter called “pleak” in a “dbfsi” ASCII file. See *DATABASE_FSI. 3. The *ALE_FSI_SWITCH_MMG_ID card track any flow across S9 and switch the AMMGSID from 125 (AMMG 1) to 126 (AMMG 3). *ALE Purpose: Output the ALE coupling forces from *CONSTRAINED_LAGRANGE_IN_- SOLID, CTYPE = 4 in keyword format, so they may be applied directly in another run. Card 1 Variable 1 DT 2 3 4 5 6 7 8 NSID IOPT Type I I Default none none I 0 VARIABLE DESCRIPTION DT NSID IOPT Output intervals Node Set ID. See *SET_NODE. Options to map the coupling data between 2 runs: EQ.0: The keyword alefsiloadnode.k is created at the end of the run by LS-DYNA. EQ.1: A database of coupling forces is dumped without the conversion in keyword file at the end of the run . The database can be treated by a program (alefsiloadnode.exe) to write alefsiloadnode.k. EQ.2: The database of coupling forces created by IOPT = 1 is read back. The structure meshes should be identical. The forces are directly applied the nodes with- out using *LOAD_NODE. The parameters DT and NSID are not read. EQ.3: A database of coupling accelerations is dumped at the end of the run . EQ.4: The database of coupling accelerations created by IOPT = 3 is read back. The structure meshes can be different. The accelerations are interpo- lated at the nodes provided by NSID. The parameters DT and NSID are read. *ALE_FSI_TO_LOAD_NODE 1. The name of the output keyword file is alefsiloadnode.k. For each node, this file contains three *LOAD_NODE for each global direction and three *DE- FINE_CURVE for the coupling force histories. 2. The name of the database is alefsi2ldnd.tmp (or alefsi2ldnd.tmp00… in MPP). It should be in the directory of the 2nd run for IOPT = 2. The database lists the coupling forces by node. The structure meshes (and their MPP decomposition) for the IOPT = 1 and IOPT = 2 runs should be the same. 3. The names of the databases are alefsi2ldnd.tmp (or alefsi2ldnd.tmp00… in MPP) and alefsi2lndndx.tmp. They should be in the directory of the 2nd run for IOPT = 4. The file alefsi2ldnd.tmp lists the coupling accelerations by node file (coupling acceleration = coupling alefsi2lndndx.tmp lists the initial nodal coordinates and coupling segment connectivities . The structure meshes for the IOPT = 3 and IOPT = 4 runs can be different. The IOPT = 3 initial geometry stored in alefsi2lndndx.tmp is used to interpolate the coupling accelerations (saved in alefsi2ldnd.tmp) at the nodes provided by NSID. For the interpolation to work, these nodes should be within the IOPT = 3 coupling segment initial locations. force / nodal mass). The *ALE_MULTI-MATERIAL_GROUP *ALE_MULTI-MATERIAL_GROUP *ALE Purpose: This command defines the appropriate ALE material groupings for interface reconstruction when two or more ALE Multi-Material Groups (AMMG) are present in a model. This card is required when ELFORM = 11 in the *SECTION_SOLID card or when ALEFORM = 11 in *SECTION_ALE1D or *SECTION_ALE2D. Each data line represents one ALE multi-material group (AMMG), with the first line referring to AM- MGID 1, second line AMMGID 2, etc. Each AMMG represents one unique “fluid” which may undergo interaction with any Lagrangian structure in the model. Card 1 1 2 3 4 5 6 7 8 Variable SID IDTYPE Type I Default none I 0 Remarks 1 VARIABLE DESCRIPTION SID Set ID. IDTYPE Set type: EQ.0: Part set, EQ.1: Part. Remarks: 1. When ELFORM = 12 in the *SECTION_SOLID card (single material and void), this card should not be used. In one model, ELFORM = 12 cannot be used to- gether with ELFORM = 11. If possible, it is recommended that ELFORM = 11 be used as it is the most robust and versatile formulation for treating multi- material ALE parts. 2. Each AMMG is automatically assigned an ID (AMMGID), and consists of one or more PART ID’s. The interface of each AMMGID is reconstructed as it evolves dynamically. Each AMMGID is represented by one material contour color in LS-PrePost. Physical Material 3 (PID 44) Physical Material 3 (PID 55) Physical Material 3 (PID 66) Physical Material 4 (PID 77) Physical Material 1 (PID 11) Physical Material 2 (PID 22) Physical Material 2 (PID 33) Figure 4-1. Schematic illustration of Example 1. 3. The maximum number of AMMGIDs allowed has been increased to 20. However, there may be 2, at most 3, AMMGs inside an ALE element at any- time. If there are more than 3 AMMGs inside any 1 ALE element, the ALE mesh needs refinement. Better accuracy is obtained with 2 AMMGs in mixed elements. 4. To plot these AMMGIDs in LS-PrePost: [FCOMP] ⇒ [MISC] ⇒ [VOLUME FRACTION OF AMMGID #] ⇒ [APPLY] (Note: Contour definitions maybe different for gas mixture application) 5. It is very important to distinguish among the a) Physical materials, b) PART IDs, and c) AMMGIDs. A *PART may be any mesh component. In ALE formulation, it is simply a geometric entity and a time = 0 concept. This means a *PART may be a mesh region that can be filled with one or more AMMGIDs at time zero, via a volume filling command (*INITIAL_VOLUME_FRACTION_GEOMETRY). An AM- MGID represents a physical material group which is treated as one material entity (represented by 1 material color contour in LS-PrePost plotting). AMMGID is used in dealing with multiple ALE or Eulerian materials. For example, it can be used to specify a master ALE group in a coupling card. Example 1: Consider a purely Eulerian model containing 3 containers containing 2 different physical materials (fluids 1 and 2). All surrounded by the background material (maybe air). The containers are made of the same material, say, metal. Assume that these containers explode and spill the fluids. We want to track the flow and possibly mixing of the various materials. Note that all 7 parts have ELFORM = 11 in their *SECTION_- SOLID cards. So we have total of 7 PIDs, but only 4 different physical materials. See Figure 4-1. Approach 1: If we want to track only the interfaces of the physical materials. $...|....1....|....2....|....3....|....4....|....5....|....6....|....7....|....8 *SET_PART 1 11 *SET_PART 2 22 33 *SET_PART 3 44 55 66 *SET_PART 4 77 *ALE_MULTI-MATERIAL_GROUP 1 0 ← 1st line = 1st AMMG ⇒AMMGID = 1 2 0 ← 2nd line = 2nd AMMG ⇒AMMGID = 2 3 0 ← 3rd line = 3rd AMMG ⇒AMMGID = 3 4 0 ← 4th line = 4th AMMG ⇒AMMGID = 4 $...|....1....|....2....|....3....|....4....|....5....|....6....|....7....|....8 With this approach, we define only 4 AMMGs (NALEGP = 4). So in LS-PrePost, when plotting the material-group (history variable) contours, we will see 4 colors, one for each material group. One implication is that when the fluids from part 22 and part 33 flow into the same element, they will coalesce and no boundary distinction between them is maintained subsequently. While this may be acceptable for fluids at similar thermodynamic states, this may not be intuitive for solids. For example, if the solid container materials from parts 44, 55 and 66 flow into one element, they will coalesce “like a single fluid”, and no interfaces among them are tracked. If this is undesirable, an alternate approach may be taken. It is presented next. Approach 2: If we want to reconstruct as many interfaces as necessary, in this case, we follow the interface of each part. $...|....1....|....2....|....3....|....4....|....5....|....6....|....7....|....8 *ALE_MULTI-MATERIAL_GROUP 1 1 ← 1st line = 1st AMMG ⇒AMMGID = 1 2 1 ← 2nd line = 2nd AMMG ⇒AMMGID = 2 3 1 ← 3rd line = 3rd AMMG ⇒AMMGID = 3 4 1 ← 4th line = 4th AMMG ⇒AMMGID = 4 5 1 ← 4th line = 5th AMMG ⇒AMMGID = 5 6 1 ← 4th line = 6th AMMG ⇒AMMGID = 6 7 1 ← 4th line = 7th AMMG ⇒AMMGID = 7 $...|....1....|....2....|....3....|....4....|....5....|....6....|....7....|....8 There are 7 AMMGs in this case (NALEGP = 7). This will involve more computational cost for the additional tracking. Realistically, accuracy will be significantly reduced if there are more than 3 or 4 materials in any one element. In that case, higher mesh resolution may be required. Example 2: Oil Water Air Group 1 Group 2 Group 3 Part IDs 1 and 2 Part ID 3 Part IDs 5, 6, and 7 The above example defines a mixture of three groups of materials (or “fluids”), oil, water and air, that is, the number of ALE multi-material groups (AMMGs) NALEGP = 3. The first group contains two parts (materials), part ID's 1 and 2. The second group contains one part (material), part ID 3. The third group contains three parts (materials), part ID's 5, 6 and 7. *ALE Purpose: This command defines a motion and/or a deformation prescribed for a geometric entity, where a geometric entity may be any part, part set, node set, or segment set. The motion or deformation is completely defined by the 12 parameters shown in the equation below. These 12 parameters are defined in terms of 12 load curves. This command is required only when PRTYPE = 3 in the *ALE_REFERENCE_- SYSTEM_GROUP command. 2 3 4 5 6 7 8 Card 1 Variable 1 ID Type I Default none Card 2 1 2 3 4 5 6 7 8 Variable LCID1 LCID2 LCID3 LCID4 LCID5 LCID6 LCID7 LCID8 Type I I I I I I I I Default none none none none none none none none Card 3 1 2 3 4 5 6 7 8 Variable LCID9 LCID10 LCID11 LCID12 Type I I I I Default none none none none VARIABLE DESCRIPTION ID Curve group ID. LCID1, …, LCID12 Load curve IDs. *ALE_REFERENCE_SYSTEM_CURVE 1. The velocity of a node at coordinate (𝑥, 𝑦, 𝑧) is defined as: {⎧𝑥̇ }⎫ 𝑦̇ 𝑧̇⎭}⎬ ⎩{⎨ = {⎧𝑓1 }⎫ 𝑓5 𝑓9⎭}⎬ ⎩{⎨ + 𝑓2 ⎡ 𝑓6 ⎢ 𝑓10 ⎣ 𝑓3 𝑓7 𝑓11 𝑓4 ⎤ 𝑓8 ⎥ 𝑓12⎦ {⎧𝑥 − XC }⎫ 𝑦 − YC 𝑧 − ZC⎭}⎬ ⎩{⎨ where 𝑓1(𝑡) is the value of load curve LCID1 at time 𝑡, 𝑓2(𝑡) is the value of load curve LCID2 at time 𝑡 and so on. The functions 𝑓1(𝑡), 𝑓5(𝑡), and 𝑓9(𝑡) respectively correspond to the translation components in global 𝑥, 𝑦, and 𝑧 direction, while the functions 𝑓2(𝑡), 𝑓7(𝑡), and 𝑓12(𝑡) correspond to and expansion or contraction along the 𝑥, 𝑦, and 𝑧 axes. The parameters XC, YC and ZC from the second data card of *ALE_REFER- ENCE_SYSTEM_GROUP define the center of rotation and expansion of the mesh. If the mesh translates, the center position is updated with 𝑓1(𝑡), 𝑓5(𝑡), and 𝑓9(𝑡). If LCID8, LCID10, LCID3 are equal to −1, their corresponding values 𝑓8(𝑡), 𝑓10(𝑡), and 𝑓3(𝑡) will be equal to −𝑓11(𝑡), −𝑓4(𝑡), and −𝑓6(𝑡) so as to make a skew symmetric matrix thereby inducing a rigid rotation of the mesh about the axis 𝐯 defined by the triple, 𝐯 = (𝑓11(𝑡), 𝑓4(𝑡), 𝑓6(𝑡)) Example: Consider a motion that consists of translation in the x and y direction only. Thus only 𝑓1(𝑡) and 𝑓5(𝑡) are required. Hence only 2 load curve ID’s need be defined: $...|....1....|....2....|....3....|....4....|....5....|....6....|....7....|...8 *ALE_REFERENCE_SYSTEM_GROUP $ SID STYPE PRTYP PRID BCTRAN BCEXP BCROT ICOORD 1 0 3 11 0 7 0 $ XC YC ZC EXPLIM 0 0 0 0 *ALE_REFERENCE_SYSTEM_CURVE $ CURVESID 11 $ LCID1 LCID2 LCID3 LCID4 LCID5 LCID6 LCID7 LCID8 111 0 0 0 222 0 0 0 $ LCID9 LCID10 LCID11 LCID12 0 0 0 0 *DEFINE_CURVE $ lcid sidr sfa sfo offa offo dattyp 111 $ a1 o1 0.00 5.0 0.15 4.0 *DEFINE_CURVE $ lcid sidr sfa sfo offa offo dattyp 222 $ a1 o1 0.00 -1.0 0.15 -5.0 $...|....1....|....2....|....3....|....4....|....5....|....6....|....7....|....8 *ALE_REFERENCE_SYSTEM_GROUP Purpose: This card is used to associate a geometric entity to a reference system type. A geometric entity may be any part, part set, node set, or segment set of a model (or a collection of meshes). A reference system type refers to the possible transformation allowed for a geometric entity (or mesh). This command defines the type of reference system or transformation that a geometric entity undergoes. In other words, it prescribes how certain mesh can translate, rotate, expand, contract, or be fixed in space, etc. Card 1 1 2 3 4 5 6 7 8 Variable SID STYPE PRTYPE PRID BCTRAN BCEXP BCROT ICR/NID Type I Default none Card 2 Variable 1 XC Type F I 0 2 YC F I 0 3 ZC F I 0 4 I 0 5 I 0 6 I 0 7 I 0 8 EXPLIM EFAC FRCPAD IEXPND F F F 0.1 I 0 Default 0.0 0.0 0.0 inf. 0.0 Remaining cards are optional.† Card 3 1 2 3 4 5 6 7 8 Variable IPIDXCL IPIDTYP Type Default I 0 I VARIABLE DESCRIPTION SID Set ID. STYPE Set type: EQ.0: part set, EQ.1: part, EQ.2: node set, EQ.3: segment set. PRTYPE Reference system type : EQ.0: Eulerian, EQ.1: Lagrangian, EQ.2: Normal ALE mesh smoothing, EQ.3: Prescribed motion following load curves, see *ALE_REF- ERENCE_SYSTEM_CURVE, EQ.4: Automatic mesh motion following mass weighted average velocity in ALE mesh, EQ.5: Automatic mesh motion following a local coordinate system defined by three user defined nodes, see *ALE_- REFERENCE_SYSTEM_NODE, EQ.6: Switching in time between different reference system types, see *ALE_REFERENCE_SYSTEM_SWITCH, EQ.7: Automatic mesh expansion in order to enclose up to twelve user defined nodes, see *ALE_REFERENCE_SYS- TEM_NODE. EQ.8: Mesh smoothing option for shock waves, where the element grid contracts in the vicinity of the shock front: this may be referred to as the Delayed-ALE option. It controls how much the mesh is to be moved during the remap step. This option requires the definition of the 5th parameter in the 2nd card, EFAC; see below for defini- tion. EQ.9: Allowing the ALE mesh(es) to: 1. Translate and/or rotate to follow a local Lagrangian reference coordinate system *ALE_REFER- ENCE_SYSTEM_NODE card ID is defined by the BC- TRAN parameter) (whose VARIABLE DESCRIPTION 2. Expand or contract to enclose a Lagrangian part-set ID defined by the PRID parameter. 3. Has a Lagrangian node ID be defined by the ICR/NID parameter to be the center of the ALE mesh expansion. PRID A parameter giving additional information depending on the reference system (PRTYPE) choice: PRTYPE.EQ.3: PRID defines a load curve group ID specifying an *ALE_REFERENCE_SYSTEM_CURVE card for mesh translation. This defines up to 12 curves which prescribe the motion of the sys- tem. PRTYPE.EQ.4: PRID defines a node set ID (*SET_NODE), for which a mass average velocity is computed. This velocity controls the mesh motion. PRTYPE.EQ.5: PRID defines a node group ID specifying an *ALE_REFERENCE_SYSTEM_NODE card, via which, three nodes forming a local coordinate system are defined. PRTYPE.EQ.6: PRID defines a switch list ID specifying an *ALE_REFERENCE_SYSTEM_SWITCH card. This defines the switch times and the reference system choices for each time interval between the switches. PRTYPE.EQ.7: PRID defines a node group ID specifying an *ALE_REFERENCE_SYSTEM_NODE card. Up to 12 nodes in space forming a region to be en- veloped by the ALE mesh are defined. PRTYPE.EQ.9: PRID defines a Lagrangian part set ID (PSID) defining the Lagrangian part(s) whose range of motion is to be enveloped by the ALE mesh(es). This is useful for airbag modeling. If PRTYPE.EQ.4 or PRTYPE.EQ.5, then BCTRAN BCTRAN is a translational constraint (Remark 3). EQ.0: no constraints, EQ.1: constrained 𝑥 translation, VARIABLE DESCRIPTION EQ.2: constrained 𝑦 translation, EQ.3: constrained 𝑧 translation, EQ.4: constrained 𝑥 and 𝑦 translation, EQ.5: constrained 𝑦 and 𝑧 translation, EQ.6: constrained 𝑧 and 𝑥 translation, EQ.7: constrained 𝑥, 𝑦, and 𝑧 translation. Else If PRTYPE.EQ.9, then BCTRAN BCTRAN is a node group ID from a *ALE_REFERENCE_SYS- TEM_NODE card prescribing a local coordinate system (3 node IDs) whose motion is to be followed by the ALE mesh(es). Else BCTRAN Ignored End if BCEXP For PRTYPE = 4 & 7 BCTRAN is an expansion constraint, otherwise it is ignored (Remark 3). EQ.0: no constraints, EQ.1: constrained 𝑥 expansion, EQ.2: constrained 𝑦 expansion, EQ.3: constrained 𝑧 expansion, EQ.4: constrained 𝑥 and 𝑦 expansion, EQ.5: constrained 𝑦 and 𝑧 expansion, EQ.6: constrained 𝑧 and 𝑥 expansion, EQ.7: constrained 𝑥, 𝑦, and 𝑧 expansion. BCROT BCROT is a rotational constraint (Remark 3). Otherwise, BCROT is ignored. EQ.0: no constraints, EQ.1: constrained 𝑥 rotation, EQ.2: constrained 𝑦 rotation, VARIABLE DESCRIPTION EQ.3: constrained 𝑧 rotation, EQ.4: constrained 𝑥 and 𝑦 rotation, EQ.5: constrained 𝑦 and 𝑧 rotation, EQ.6: constrained 𝑧 and 𝑥 rotation, EQ.7: constrained 𝑥, 𝑦, and 𝑧 rotation. If PRTYPE.EQ.4 ICR/(NID) ICR is a flag the specifies the method LS-DYNA uses for determining the center point for expansion and rotation (Remark 3). EQ.0: The center is at center of gravity of the ALE mesh. EQ.1: The center is at (XC, YC, ZC), just a point in space (it does not have to be a defined node) Else if PRTYPE.EQ.9 (ICR)/NID NID sets the Lagrangian node ID for the node that anchors the center of ALE mesh expansion (Remark 2). End if XC, YC, ZC EXPLIM Center of mesh expansion and rotation for PRTYPE = 4 and 5, otherwise ignored. See ICR above. Limit ratio for mesh expansion and contraction. Each Cartesian direction is treated separately. The distance between the nodes is not allowed to increase by more than a factor EXPLIM, or decrease to less than a factor 1/EXPLIM. This flag applies only for PRTYPE = 4, otherwise it is ignored. EFAC Mesh remapping factor for PRTYPE = 8 only, otherwise it is ignored. EFAC is allowed to range between 0.0 and 1.0. When EFAC approaches 1.0, the remapping approaches the Eulerian behavior. The smaller the value of EFAC, the closer the mesh will follow the material flow in the vicinity of a shock front, i.e. approaching Lagrangian behavior. Note that excessively small values for EFAC can result in severe VARIABLE DESCRIPTION FRCPAD mesh distortions as the mesh follows the material flow. As time evolves, the mesh smoothing behavior will approach that of an Eulerian system. For PRTYPE = 9 this is an ALE mesh padding fraction, otherwise it is ignored. FRCPAD is allowed to range from 0.01 to 0.2. If the characteristic Lagrange mesh dimension, 𝑑𝐿1, exceeds (1 − 2 × FRCPAD) × 𝑑𝐿𝐴, where 𝑑𝐿𝐴 is the characteristic length of the ALE mesh, then the ALE mesh is expanded so that 𝑑𝐿𝐴 = 𝑑𝐿1 1 − 2 × FRCPAD . This provides an extra few layers of ALE elements beyond the maximum Lagrangian range of motion. EQ.0.01: 𝑑𝐿𝐴 = EQ.0.20: 𝑑𝐿𝐴 = 𝑑𝐿𝐿 ⁄ 0.98 𝑑𝐿𝐿 ⁄ 0.60 = 𝑑𝐿𝐿 × 1.020408 = 𝑑𝐿𝐿 × 1.666667 IEXPND For PRTYPE = 9 this is an ALE mesh expansion control flag, otherwise it is ignored. EQ.0: Both mesh expansion and contraction are allowed. EQ.1: Only mesh expansion is allowed: IPIDXCL An ALE set ID to be excluded from the expansion and/or contraction only. Translation and rotation are allowed. For example, this may be used to prevent the ALE mesh (or part) at the inflator gas inlet region from expanding too much. High ALE mesh resolution is usually required to resolve the high speed flow of the gas into the airbag via point sources . IPIDTYPE Set ID type of IPIDXCL: EQ.0: PSID EQ.1: PID *ALE_REFERENCE_SYSTEM_GROUP 1. Required Associated Cards. Some PRTYP values may require a supple- mental definition defined via corresponding PRID. For example, PRTYP = 3 requires a *ALE_REFERENCE_SYSTEM_CURVE card. If PRID = n, then in the corresponding *ALE_REFERENCE_SYSTEM_CURVE card, ID = n. Similar association applies for any PRTYP (i.e. 3, 5, 6, or 7) which requires a definition for its corresponding PRID parameter. 2. Mesh Centering. For PRTYPE = 9: ICR/NID can be useful to keep a high density ALE mesh centered on the region of greatest interest, (such as the in- flator orifices region in an airbag model). For example, in the case of nonsym- metrical airbag deployment, assuming that the ALE mesh is initially finer near the inlet orifices, and gradually coarsened away from it. Defining an “anchor node” at the center of the orifice location will keep the fine ALE mesh region centered on the orifice region. So that this fine ALE mesh region will not be shifted away (from the point sources) during expansion and translation. The ALE mesh can move and expand outward to envelop the Lagrangian airbag in such a way that the inlet is well resolved throughout the deployment. 3. Additional Constraints. The table below shows the applicability of the various choices of PRTYPE. Simple deductions from the functional definitions of the PRTYPE choices will clarify the applications of the various constraints. For example, when PRTYP = 3, nodal motion of the ALE mesh is completely con- trolled by the 12 curves. Therefore, no constraints are needed. PRTYPE ICR/NID BCTRAN BCROT BCEXP 3 4 5 6 7 8 9 NO YES (ICR) NO NO NO NO NO YES YES NO NO NO YES (NID) YES (NGID) NO YES NO NO NO NO NO NO YES NO NO YES NO NO Example 1: Consider a bird-strike model containing 2 ALE parts: a bird is surrounded by air (or void). A part-set ID 1 is defined containing both parts. To allow for the meshes of these 2 parts to move with their combined mass-weighted-average velocity, PRTYPE = 4 is used. Note that BCEXP = 7 indicating mesh expansion is constrained in all global directions. $...|....1....|....2....|....3....|....4....|....5....|....6....|....7....|...8 *ALE_REFERENCE_SYSTEM_GROUP $ SID STYPE PRTYP PRID BCTRAN BCEXP BCROT ICOORD 1 0 4 0 0 7 0 $ XC YC ZC EXPLIM 0 0 0 0 $...|....1....|....2....|....3....|....4....|....5....|....6....|....7....|...8 Example 2: Consider a bouncing ball model containing 2 ALE parts: a solid ball (PID 1) is surrounded by air or void (PID 2). A part-set ID 1 is defined containing both parts. To allow for the meshes of these 2 parts to move with 2 reference system types: (a) first, they move with their combined mass-weighted-average velocity between 0.0 and 0.01 second; and subsequently (between 0.01 and 10.0 seconds) their reference system is switched to (b) an Eulerian system (thus the mesh is fixed in space), a reference system “SWITCH” is required. This is done by setting PRTYPE = 6. This PRTYPE requires a corresponding *ALE_REFERENCE_SYSTEM_SWITCH card. Note that PRID = 11 in the *ALE_REFERENCE_SYSTEM_GROUP card corresponds to the SWITCHID = 11 in *ALE_REFERENCE_SYSTEM_SWITCH card. $...|....1....|....2....|....3....|....4....|....5....|....6....|....7....|....8 *ALE_REFERENCE_SYSTEM_GROUP $ SID STYPE PRTYP PRID BCTRAN BCEXP BCROT ICOORD 1 0 6 11 0 7 7 $ XC YC ZC EXPLIM EULFACT SMOOTHVMX 0 0 0 0 0.0 *ALE_REFERENCE_SYSTEM_SWITCH $ SWITCHID 11 $ t1 t2 t3 t4 t5 t6 t7 0.01 10.0 $ TYPE1 TYPE2 TYPE3 TYPE4 TYPE5 TYPE6 TYPE7 TYPE8 4 0 $ ID1 ID2 ID3 ID4 ID5 ID6 ID7 ID8 0 0 0 0 0 0 0 0 $...|....1....|....2....|....3....|....4....|....5....|....6....|....7....|....8 *ALE_REFERENCE_SYSTEM_NODE Purpose: This command defines a group of nodes that control the motion of an ALE mesh. It is used only when PRTYPE = 5 or 7 in a corresponding *ALE_REFERENCE_- SYSTEM_GROUP card. 2 3 4 5 6 7 8 Card 1 Variable 1 ID Type I Default none Card 2 1 2 3 4 5 6 7 8 Variable NID1 NID2 NID3 NID4 NID5 NID6 NID7 NID8 Type I I I I I I I I Default none none none none none none none none Card 3 1 2 3 4 5 6 7 8 Variable NID9 NID10 NID11 NID12 Type I I I I Default none none none none VARIABLE DESCRIPTION ID Node group ID for PRTYPE 5 or 7, see *ALE_REFERENCE_SYS- TEM_GROUP. User specified nodes. NID1, …, NID12 Remarks: 1. For PRTYPE = 5 the ALE mesh is forced to follow the motion of a coordinate system, which is defined by three nodes (NID1, NID2, NID3). These nodes are located at 𝑥1, 𝑥2 and 𝑥3, respectively. The axes of the coordinate system, 𝑥′, 𝑦′, and 𝑧′, are defined as: 𝑥′ = 𝑥2 − 𝑥1 |𝑥2 − 𝑥1| 𝑦′ = 𝑧′ × 𝑥′ 𝑧′ = 𝑥′ × 𝑥3 − 𝑥1 ∣𝑥′ × (𝑥3 − 𝑥1)∣ Note that 𝑥1 → 𝑥2 is the local 𝑥′axis, 𝑥1 → 𝑥3 is the local 𝑦′ axis and 𝑥′ crosses 𝑦′ gives the local 𝑧′ axis. These 3 nodes are used to locate the reference system at any time. Therefore, their positions relative to each other should be as close to an orthogonal system as possible for better transformation accuracy of the ALE mesh. 2. For PRTYPE = 7, the ALE mesh is forced to move and expand, so as to enclose up to twelve user defined nodes (NID1, …, NID12). This is a rarely used op- tion. Example 1: Consider modeling sloshing of water inside a rigid tank. Assuming there are 2 ALE parts, the water (PID 1) and air or void (PID 2) contained inside a rigid (Lagrangian) tank (PID 3). The outer boundary nodes of both ALE parts are merged with the inner tank nodes. A part-set ID 1 is defined containing both ALE parts (PIDs 1 and 2). To allow for the meshes of the 2 ALE parts to move with the rigid Lagrangian tank, PRTYPE = 5 is used. The motion of the ALE parts then follows 3 reference nodes on the rigid tank. These 3 reference nodes must be defined by a corresponding *ALE_REFER- ENCE_SYSTEM_NODE card. In this case the reference nodes have the nodal IDs of 5, 6 and 7. Note that PRID = 12 in the *ALE_REFERENCE_SYSTEM_GROUP card corresponds to the SID = 12 in the *ALE_- REFERENCE_SYSTEM_NODE card. $...|....1....|....2....|....3....|....4....|....5....|....6....|....7....|...8 *ALE_REFERENCE_SYSTEM_GROUP $ SID STYPE PRTYP PRID BCTRAN BCEXP BCROT ICOORD 1 0 5 12 $ XC YC ZC EXPLIM 0 0 0 0 *ALE_REFERENCE_SYSTEM_NODE $ NSID 12 $ N1 N2 N3 N4 N5 N6 N7 N8 5 6 7 $...|....1....|....2....|....3....|....4....|....5....|....6....|....7....|...8 *ALE_REFERENCE_SYSTEM_SWITCH Purpose: The PRTYPE parameter in the *ALE_REFERENCE_SYSTEM_GROUP (ARSG) card allows many choices of the reference system types for any ALE geometric entity. This command allows for the time-dependent switches between these different types of reference systems, i.e., switching to multiple PRTYPEs at different times during the simulation. This command is required only when PRTYPE = 6 in ARSG card. Please see example 2 in the ARSG section. 2 3 4 5 6 7 8 Card 1 Variable 1 ID Type I Default none Card 2 Variable 1 T1 Type F 2 T2 F 3 T3 F 4 T4 F 5 T5 F 6 T6 F 7 T7 F 8 Default 0.0 0.0 0.0 0.0 0.0 0.0 0.0 Card 3 1 2 3 4 5 6 7 8 Variable TYPE1 TYPE2 TYPE3 TYPE4 TYPE5 TYPE6 TYPE7 TYPE8 Type Default I 0 I 0 I 0 I 0 I 0 I 0 I 0 I Card 4 1 Variable ID1 2 ID2 3 ID3 4 ID4 5 ID5 6 ID6 7 ID7 8 ID8 Type I I I I I I I I Default none none none none none none none none VARIABLE DESCRIPTION ID Switch list ID, see *ALE_REFERENCE_SYSTEM_GROUP, T1, …, T7 TYPE1, …, TYPE8 Times for switching reference system type. By default, the reference system TYPE1 occurs between time = 0 and time = T1, and TYPE2 occurs between time = T1 and time = T2, etc. Reference system types (also see PRTYPE under ARSG): EQ.0: Eulerian, EQ.1: Lagrangian, EQ.2: Normal ALE mesh smoothing, EQ.3: Prescribed motion following load curves, see *ALE_REF- ERENCE_SYSTEM_CURVE, EQ.4: Automatic mesh motion following mass weighted average velocity in ALE mesh, EQ.5: Automatic mesh motion following a local coordinate system defined by three user defined nodes, see *ALE_- REFERENCE_SYSEM_NODE, ID1, …, ID8 The corresponding PRID parameters supporting each PRTYPE used during the simulation. Remarks: 1. The beginning time is assumed to be t = 0, and the starting PRTYPE is TYPE1. So at T1, the 1st switching time, PRTYPE is switched from TYPE1 to TYPE2, and so forth. This option can be complex in nature so it is seldom applied. See *CONTROL_REFINE_ALE. *ALE *ALE_SMOOTHING Purpose: This smoothing constraint keeps an ALE slave node at its initial parametric location along a line between two other ALE nodes. If these nodes are not ALE nodes, the slave node has to follow their motion . This constraint is active during each mesh smoothing operation. This keyword can be used with ALE solids, ALE shells and ALE beams. Card 1 1 2 3 4 5 6 7 8 Variable SNID MNID1 MNID2 IPRE XCO YCO ZCO Type I I I Default none none none I 0 F F F 0.0 0.0 0.0 VARIABLE DESCRIPTION SNID Slave ID, see Figure 4-2. GT.0: SNID is an ALE node, EQ.0: the slaves are the nodes of an ALE mesh connected to the first master nodes (MNID1). See Remarks 2 and 4. LT.0: |SNID| is a ID of ALE node set. See Remark 2. 1st master node slave node Figure 4-2. This simple constraint, which ensures that a slave node remains on a straight line between two master nodes, is sometimes necessary during ALE smoothing. 2nd master node VARIABLE DESCRIPTION MNID1 First master ID. GT.0: MNID1 is a node, LT.0: |MNID1| is if XCO = YCO = ZCO = 0.0. Otherwise, |MNID1| is a node set ID. See Remarks 2 and 3. segment set ID a MNID2 Second master ID. GT.0: MNID2 is a node, EQ.0: the slave motion is solely controlled by MNID1. See Remark 5. LT.0: |MNID2| is a node set ID. See Remark 2. IPRE EQ.0: smoothing constraints are performed after mesh relaxation, EQ.1: smoothing constraints are performed before mesh relaxation. 𝑥-coordinate of constraint vector 𝑦-coordinate of constraint vector 𝑧-coordinate of constraint vector XCO YCO ZCO Remarks: 1. When Master Nodes Are Not ALE Nodes. If SNID, MNID1 and MNID2 are ALE nodes, the positions of MNID1 and MNID2 are interpolated to position SNID. If MNID1 and MNID2 are not ALE nodes, the motions of MNID1 and MNID2 are interpolated to move SNID. 2. Node Sets for Constraint Generation. If MNID1 is a set, SNID and MNID2 should be node sets or zeros. In such a case, the constraints are created during the initialization and printed out in a file called alesmoothingenerated.k for the user’s convenience. 3. Constraint Generation Algorithm. The constraints for a given master node in MNID1 are generated by finding the closest slave nodes to an axis passing through the constraint vector (XCO,YCO,ZCO) if MNID1 is a node set. If MNID1 is a segment set, the nor- the master node and oriented by mals of the segments connected to the master node are averaged to give a direc- tion to the axis. 4. Automatic Identification of Slave Nodes. If SNID=0, MNID1 should be a set of nodes or segments along the boundary of an ALE mesh. For a given master node in MNID1, the constraints are created for all the nodes of the mesh found the closest to the axis described previously. The search of slaves starts with nodes of elements connected to the master node and stops when a boundary node with an element connectivity similar to the master node’s one is reached or when a node in the set MNID2 (if defined) is found. 5. MNID2 = 0. If MNID2=0 and SNID is defined, MNID1 should not be ALE. Otherwise SNID and MNID1 positions would match and the element volumes between them could be zero or negative. Only SNID and MNID1 motion should match in such a case. *ALE Purpose: This keyword generates a structured 3D mesh and invokes the Structured ALE (S-ALE) solver. Spacing parameters are input through one or more of the *ALE_- STRUCTURED_MESH_CONTROL_POINTS cards. The local coordinate system is defined using the *ALE_STRUCTURED_MESH card. In certain contexts it is advantageous to use structured meshes. With structured meshes the element and node connectivity are straightforward and the searching algorithm used for ALE coupling is greatly simplified. Also numerous checks are avoided because these meshes include only HEX elements. This new S-ALE solver supports SMP, MPP and MPP hybrid configurations. All three implementations require less simulation time and memory usage than the regular ALE solver. We, therefore, encourage using the S-ALE solver when the ALE mesh is structured. The S-ALE solver uses the same set of keyword cards as the regular ALE solver with the only exception being this keyword. Once an ALE mesh is generated using *ALE_- STRUCTURED_MESH card this card invokes the S-ALE and performs the ALE advection timestep. For fluid structured interaction using the *CONSTRAINED_- LARGANGE_IN_SOLID card S-ALE uses a much faster searching algorithm that takes advantage of the mesh structure. Card 1 1 2 3 4 5 6 7 8 Variable MSHID DPID NBID EBID Type Default I 0 I none Card 2 1 2 I 0 3 I 0 4 5 6 7 8 Variable CPIDX CPIDY CPIDZ NID0 LCSID Type I I I I I Default none none none none none VARIABLE DESCRIPTION MSHID DPID NBID EBID CPIDX, CPIDY, CPIDZ S-ALE Mesh ID. A unique number must be specified. Default Part ID. The elements generated will assigned to DPID. This part contains no material including only the mesh. is automatically generated during the input phase and contains neither material nor element formulation information. Please see Remark 1. This part definition Nodes are generated and assigned with node IDs starting from NBID. Elements are generated and assigned with element IDs starting from EBID. Control point IDs defining node ID/value pairs along each local axis. See *ALE_STRUCTURED_MESH_- CONTROL_POINTS. NID0 During the NID0 sets the mesh’s origin node. simulation, prescribed motion applied to this node applies to the entire structure S-ALE mesh. LCSID Local coordinate system ID. Please see Remark 2. Remarks: 1. DPID. The part specific by ID DPID wholey consists of elements and nodes. It does not include material properties or integration rules. The requirmenet that a part ID be specified for these automatically generated S-ALE solid elements exusts only to satisfy the legacy rule that every element must be associated with a part. Users do not need to set up the *PART card for DPID. All PART defini- tions used in this card only refer to mesh, not material. 2. LCSID. The local coordinate system is defined on the data cards associated with the *DEFINE_COORDINATE keyword. This local coordinate cordinate system specifies the three cardinal directions used for generating the structured ALE mesh. The structured mesh can be made to rotate by specifying a rotating local coordinate system. To define a rotating local coordinate system, use the *DEFINE_COORDINATE_NODES keyword with FLAG = 1 and then apply prescribed motion to the three coordinate nodes. 3. ALES-ALE Converter. For existing ALE models with rectilinear mesh, we could use *ALE_STRUCTURED_MESH card to invoke the ALE S-ALE con- verter. To invoke this feature, add a *ALE_STRUCTURED_MESH card in the model input with CPIDX=-1/0 and all other fields blank. It will then convert all ALE keywords to be of S-ALE format and write the modified input in a file named “saleconvrt.inc”. The solver used to perform the analysis depends on the value of CPIDX. If -1, S-ALE solver is used; if 0, ALE solver is used. Example: The following example generates a regular evenly distributed 0.2 by 0.2 by 0.2 box mesh having 22 nodes along each direction. The generated mesh is aligned to the local coordinate system spefied by nodes 1, 2, 3, and 4 originating from node 1. All the elements inside the mesh are assigned to part 1. Note that part 1 is not explicitly defined in the input. The necessary part definition is automatically generated and contains neither material definitions nor integration rules. *ALE_STRUCTURED_MESH $ mshid dpid nbid ebid 1 1 200001 200001 $ cpidx cpidy cpidz nid0 lcsid 1001 1001 1001 1 234 *DEFINE_COORDINATE_NODES $ cid nid1 nid2 nid3 flag 234 2 3 4 1 *ALE_STRUCTURED_MESH_CONTROL_POINTS 1001 $ x1 x2 1 .0 22 .2 *NODE 1 0.0000000e+00 0.0000000e+00 0.0000000e+00 2 0.0000000e+00 0.0000000e+00 0.0000000e+00 3 0.1000000e+00 0.0000000e+00 0.0000000e+00 4 0.0000000e+00 0.1000000e+00 0.0000000e+00 *END *ALE_STRUCTURED_MESH_CONTROL_POINTS Purpose: The purpose of this keyword is to provide spacing information used by the *ALE_STRUCTURED_MESH keyword to generate a 3D structured ALE mesh. Each instance of the *ALE_STRCUTURED_MESH_CONTROL_POINTS card defines a one-dimensional mesh using control. Each control point consists of a node number and of a coordinate . The first control point must be node 1, and the node number of the last point defines the total number of nodes. Between and two control points the mesh is uniform. The *ALE_STRUCTURED_MESH card, in turn, defines a simple three dimensional mesh from the triple product of three *ALE_STRUC- TURED_MESH_CONTROL_POINT one-dimensional meshes. Card 1 1 2 3 4 5 6 7 8 Variable CPID Not used Not used SFO Not used OFFO Type I Default None F 1. F 0. Point Cards. Put one pair of points per card (2E20.0). Input is terminated at the next keyword (“*”) card. At least two cards are required, one of which, having N = 1 is required. Card 2 1 2 3 4 5 6 7 8 Variable N X RATIO Type I20 E20.0 E20.0 Default none none 0.0 VARIABLE DESCRIPTION CPID SFO Control Points ID. A unique number must be specified. This ID is to be referred in the three fields marked up CPIDX, CPIDY, CPIDZ in *ALE_STRUCTURED_MESH. Scale factor for ordinate value. This is useful for simple modifications. EQ.0.0: default set to 1.0. VARIABLE DESCRIPTION OFFO Offset for ordinate values. See Remark 1. Control point node number. Control point position. Ratio for progressive mesh spacing. Progressively larger or smaller mesh will be generated between the control point that has nonzero ratio specified and the control point following it. See remark 2. GT.0.0: mesh size increases; 𝑑𝑙𝑛+1 = 𝑑𝑙𝑛 ∗ (1 + 𝑟𝑎𝑡𝑖𝑜) LT.0.0: mesh size decreases; 𝑑𝑙𝑛+1 = 𝑑𝑙𝑛/(1 − 𝑟𝑎𝑡𝑖𝑜) N X RATIO Remarks: 1. Coordinates scaling. The ordinate values are scaled after the offsets are applied, i.e.: Ordinate value = SFO × (Defined value + OFFO) 2. Progressive mesh spacing. The formula used to calculate element length is as follows: 𝑑𝑙𝑏𝑎𝑠𝑒 = ∣𝑥𝑒𝑛𝑑 − 𝑥𝑠𝑡𝑎𝑟𝑡∣ ∗ (𝑓𝑎𝑐𝑡𝑜𝑟 − 1)/(𝑓𝑎𝑐𝑡𝑜𝑟𝑛 − 1) in which 𝑑𝑙𝑏𝑎𝑠𝑒 is the smallest base length; 𝑥𝑠𝑡𝑎𝑟𝑡 and 𝑥𝑒𝑛𝑑 are the coordinate of the start and end point 𝑓𝑎𝑐𝑡𝑜𝑟 = 1 + 𝑟𝑎𝑡𝑖𝑜 (𝑟𝑎𝑡𝑖𝑜 > 0) 𝑜𝑟 1/(1 − 𝑟𝑎𝑡𝑖𝑜) (𝑟𝑎𝑡𝑖𝑜 < 0). Please note here element size either increases by 𝑟𝑎𝑡𝑖𝑜 (𝑟𝑎𝑡𝑖𝑜 > 0) or decreases by −𝑟𝑎𝑡𝑖𝑜/(1 − 𝑟𝑎𝑡𝑖𝑜) (𝑟𝑎𝑡𝑖𝑜 < 0) each time. But the overall effect is the same: start- ing from the smallest element, each time the element size is increased by |𝑟𝑎𝑡𝑖𝑜|. respectively; Example: 1. This example below generates a regular box mesh. Its size is 0.2 by 0.2 by 0.2. It is generated in a local coordinate system defined by three nodes 2, 3, 4 and originates from node 1. The local 𝑥-axis mesh spacing is defined by control points ID 1001. It has 21 nodes evenly distributed from 0.0 to 0.2. The local 𝑦-axis is defined by ID 1002 and has twice the elements of 1001. It has 41 nodes evenly distributed from 0.0 to 0.2. The local 𝑧-axis is defined by ID 1003. It has 31 nodes and covers from 0.0 to 0.2. The mesh is two times finer in the region between node 6 and node 26. *ALE_STRUCTURED_MESH $ mshid dpid nbid ebid 1 1 200001 200001 $ cpidx cpidy cpidz nid0 lcsid 1001 1002 1003 1 234 *DEFINE_COORDINATE_NODES $ cid nid1 nid2 nid3 234 2 3 4 *ALE_STRUCTURED_MESH_CONTROL_POINTS 1001 $ x1 x2 1 .0 21 .2 *ALE_STRUCTURED_MESH_CONTROL_POINTS 1002 $ x1 x2 1 .0 41 .2 *ALE_STRUCTURED_MESH_CONTROL_POINTS 1003 $ x1 x2 1 .0 6 .05 26 .15 31 .2 *NODE 1 0.0000000e+00 0.0000000e+00 0.0000000e+00 2 0.0000000e+00 0.0000000e+00 0.0000000e+00 3 0.1000000e+00 0.0000000e+00 0.0000000e+00 4 0.0000000e+00 0.1000000e+00 0.0000000e+00 *END 2. This example shows how to generate a progressive larger/smaller mesh spacing. The mesh geometry is the same as the example above. At 𝑥-direction the mesh is progressively smaller between node 1 and 8. For these 7 elements, each element is 0.1/1.1 = 9.09% smaller than its left neighbor. Between node 15 and node 22, the mesh is progressively larger by 10% each time in those 7 elements. The 7 elements in the middle between node 8 and 15 are of equal length. *ALE_STRUCTURED_MESH $ mshid dpid nbid ebid 1 1 200001 200001 $ cpidx cpidy cpidz nid0 lcsid 1001 1002 1003 1 234 *DEFINE_COORDINATE_NODES $ cid nid1 nid2 nid3 234 2 3 4 *ALE_STRUCTURED_MESH_CONTROL_POINTS 1001 $ x1 x2 ratio 1 .0 -0.1 8 0.06666667 15 0.13333333 0.1 22 .2 *ALE Purpose: This keyword is to provide a convenient utility to refine existing meshes generated by *ALE_STRUCTURED_MESH card. All the NODESET, ELEMENTSET and SEGMENTSET defined using SALECPT and SALEFAC options in *SET_cards will be automatically updated. This way, this card is the only modification in the input deck for users to define a refined S-ALE mesh. 5 6 7 8 Card 1 1 2 Variable MSHID IFX Type I Default none I 1 3 IFY I 1 4 IFZ I 1 VARIABLE MSHID IFX, IFY, IFZ Remarks: DESCRIPTION S-ALE Mesh ID. The ID of the Structured ALE mesh to be refined. Refinement factor at each local direction. Please see remark 1. 1. IFX, IFY, IFZ prescribe how many times to refine the grid along each direction. They have to be integers. 2. This keyword provides a new modeling technique to handle the multi-material ALE problems. Compared to pure Lagrange problems, models contain multi- material ALE fluids are often time consuming and memory demanding. So it is better to construct a concept model with much coarse mesh to get an estimate of the computational resources needed and refine the concept model mesh gradu- ally until convergence is achieved. This keyword minimized the user effort following such procedure. Example: This example below generates two regular evenly distributed box mesh. Each has 22 nodes along each direction and the overall size is 0.2 by 0.2 by 0.2. S-ALE mesh 1 is generated in a local coordinate system defined by three nodes 2,3,4 and originated from node 1. If at later times, we decided to make the mesh finer, we can simply add the following card. Now the solid element set 100 would contain elements ranging between nodes (1,1,23) and (45,45,45) instead of the original (1,1,11) and (22,22,22). *ALE_STRUCTURED_MESH_REFINE $ mshid ifx ify ifz 1 2 2 2 *ALE_STRUCTURED_MESH $ mshid dpid nbid ebid 1 1 200001 200001 $ cpidx cpidy cpidz nid0 lcsid 1001 1001 1001 1 234 *DEFINE_COORDINATE_NODES $ cid nid1 nid2 nid3 234 2 3 4 *SET_SOLID_GENERAL $ SID 100 $ OPTION MSHID XMN XMX YMN YMX ZMN ZMX SALECPT 1 1 22 1 22 11 22 *ALE_STRUCTURED_MESH_CONTROL_POINTS 1001 $ x1 x2 1 .0 22 .2 *NODE 1 0.0000000e+00 0.0000000e+00 0.0000000e+00 2 0.0000000e+00 0.0000000e+00 0.0000000e+00 3 0.1000000e+00 0.0000000e+00 0.0000000e+00 4 0.0000000e+00 0.1000000e+00 0.0000000e+00 5 0.0000000e+00 0.0000000e+00 0.0000000e+00 *END *ALE Purpose: This card changes a fraction of an ALE multi-material-group (AMMGID) into another group. The fraction is to be specified by a *DEFINE_FUNCTION function. The function take as many arguments as there are fields specified on the cards in format 2. Card 1 1 2 3 4 5 6 7 8 Variable FR_MMG TO_MMG IDFUNC IDSEGSET IDSLDSET NCYCSEG NCYCSLD Type I I I Default none none None I 0 I 0 I I 50 50 Variable Cards. Cards defining the function arguments. Include as many cards as necessary. This input ends at the next keyword (“*”) card. Card 2 1 2 3 4 5 6 7 8 Variable VAR VAR VAR VAR VAR VAR VAR VAR Type Default I 0 I 0 I 0 I 0 I 0 I 0 I 0 I 0 VARIABLE FR_MMG TO_MMG DESCRIPTION This is the AMMG-SID before the switch. The AMMG-SID corresponds to the SID defined on a *SET_MULTI-MATERIAL_- GROUP_LIST (SMMGL) card. This SID refers to one or more AMMGs. See Remark 1. This is the AMMG-SID after the switch. The AMMG-SID corresponds to the SID defined on a *SET_MULTI-MATERIAL_- GROUP_LIST card. This SID refers to one or more AMMGs. See Remark 1. IDFUNC ID of a *DEFINE_FUNCTION function. This function determines the material fraction to be switched. See Example 1. IDSEGSET IDSLDSET NCYCSEG NCYCSLD *ALE_SWITCH_MMG DESCRIPTION ID of *SEGMENT_SET that is used to pass geometric properties to the function specified by IDFUNC. This field is optional. The segment center positions and normal vectors are computed. For each ALE element, this data is passed to the function IDFUNC for the segment the closest to the element center. See Example 2. The ID of a *SOLID_SET specifying which elements are affected by this particular instance of the *ALE_SWITCH_MMG keyword. This field is optional. If undefined, *ALE_SWITCH_MMG affects all ALE elements. The element centers are computed and can be used as variables in the function IDFUNC. Number of cycles between each update of the segment centers and normal vectors (if a segment set is defined). For each update, a bucket sort is applied to find the closest segment to each ALE element. If the segment nodes are fully constrained, the segment centers and normal vectors are computed only one time. Number of cycles between each update of the ALE element centers. For each update, a bucket sort is applied to find the closest segment to each ALE element. If the element nodes does not move (as with AFAC = -1 in *CONTROL_ALE) the element centers are computed exactly once. VAR Variable rank in the following list : EQ.0: EQ.1: EQ.2: EQ.3: EQ.4: EQ.5: EQ.6: EQ.7: EQ.8: EQ.9: See Remark 3 𝑥𝑥-stress for FR_MMG 𝑦𝑦-stress for FR_MMG 𝑧𝑧-stress for FR_MMG 𝑥𝑦-stress for FR_MMG 𝑦𝑧-stress for FR_MMG 𝑧𝑥-stress for FR_MMG plastic strain for FR_MMG internal energy for FR_MMG bulk viscosity for FR_MMG EQ.10: volume from previous cycle for FR_MMG GE.11 and LE.20: other auxiliary variables for FR_MMG VARIABLE DESCRIPTION GE.21 and LE.40: auxiliary variables for TO_MMG (𝑥𝑥- stress, …) EQ.41: EQ.42: EQ.43: EQ.44: EQ.45: EQ.46: EQ.47: EQ.48: EQ.49: EQ.50: EQ.51: EQ.52: EQ.53: EQ.54: EQ.55: EQ.56: EQ.57: mass for FR_MMG mass for TO_MMG volume fraction for FR_MMG volume fraction for TO_MMG material volume for FR_MMG material volume for TO_MMG time cycle 𝑥-position of the ALE element center 𝑦-position of the ALE element center 𝑧-position of the ALE element center 𝑥-position of the segment center 𝑦-position of the segment center 𝑧-position of the segment center 𝑥-component of the segment normal 𝑦-component of the segment normal 𝑧-component of the segment normal GE.58 and LE.65: 𝑥-positions of the ALE nodes GE.66 and LE.69: 𝑥-positions of the segment nodes GE.70 and LE.77: 𝑦-positions of the ALE nodes GE.79 and LE.81: 𝑦-positions of the segment nodes GE.83 and LE.89: 𝑧-positions of the ALE nodes GE.90 and LE.93: 𝑧-positions of the segment nodes GE.94 and LE.101: 𝑥-velocities of the ALE nodes GE.102 and LE.105: 𝑥-velocities of the segment nodes GE.106 and LE.113: 𝑦-velocities of the ALE nodes GE.114 and LE.117: 𝑦-velocities of the segment nodes GE.118 and LE.125: 𝑧-velocities of the ALE nodes GE.126 and LE.129: 𝑧-velocities of the segment nodes VARIABLE DESCRIPTION GE.130 and LE.137: 𝑥-accelerations of the ALE nodes GE.138 and LE.141: 𝑥-accelerations of the segment nodes GE.142 and LE.149: 𝑦-accelerations of the ALE nodes GE.150 and LE.153: 𝑦-accelerations of the segment nodes GE.154 and LE.161: 𝑧-accelerations of the ALE nodes GE.162 and LE.165: 𝑧-accelerations of the segment nodes GE.166 and LE.173: masses of the ALE nodes GE.174 and LE.177: masses of the segment nodes EQ.178: EQ.179: EQ.180: rank of the variable updated by the function rank of the multi-material group in the set time step Remarks: 1. Mapping. The multi-material group sets that are specified by the fields FR_MMG and TO_MMG must be of the same length. Multi-material groups are switched so that, for instance, the fourth multi-material group in the set FR_MMG is mapped to the fourth multi-material group in the set TO_MMG. . 2. Variable Specification. The variables are presented to the function IDFUNC as floating point data. The order of the arguments appearing in the *DEFINE_- FUNCTION should match the order of variable ranks VAR specified on Card 2 (for this keyword). For example, when there is one card in format 2 containing “47, 48, 41, 42”, then the time (47), the cycle (48), and the masses (41 & 42) should be the first, second, third, and fourth arguments to the function defined on the *DEFINE_FUNCTION keyword. If there is a blank column between 2 variable ranks, the list between these 2 ranks is specified. For example, if the card contains “1, ,6”, then the 6 stresses (1 through 6) are selected as arguments . In the case that there are several groups in the sets, if a variable rank VAR is repeated, the correspond- ing variable will be defined in the function for each group. For instance, if the sets have 3 groups and the volume fractions of the 2 first groups in the set TO_MMG are required as arguments of the function, a card in format 2 should have “44,44”. 3. Variable Update for Several Groups. If there is more than one group in the set, the function is called for each group. For a given group with a rank in the set > 1 (VAR=179), some variables including the volume fraction, mass, internal energy may have been updated during the previous switches. If their original values are required, they can be obtained by setting the first field (VAR) to 0. 4. Variable Update by the User. The variables can be updated by the user. If VAR < 0 for some variables, the function is called again (after the switch) for each of these variables. VAR = 178 gives the rank of the variable for which the function is called. The function’s return value is taken as the new value for this variable (instead of the fraction of material to switch). If the rank given by VAR = 178 is zero, it means that the function is called for the switch. Only the 46 first variables 1 < VAR < 46, 58 < VAR < 165 and VAR = 180 can be modified. Example 1: The first example switches the material if the pressure is lower than a given value. *comment units: mks Switch from the 3rd group to the 5th one if the pressure of the 3rd group is lower than pc : pres < pc Do the same for the switch from 4th to 7th If the switch occurs, the function frac returns 1.0. So the whole material is permuted. xxsig : xx-stress of the groups in the 1st *set_multi- material_group_list yysig : yy-stress of the groups in the 1st *set_multi- material_group_list zzsig : zz-stress of the groups in the 1st *set_multi- material_group_list pres : pressure pc : pressure cutoff *ALE_SWITCH_MMG $# fr_mmg to_mmg idfunc idsegset idsldset ncycseg ncycsld 1 2 10 1 2 3 *set_multi-material_group_list 1 3,4 *set_multi-material_group_list 2 5,7 *DEFINE_FUNCTION 10 float frac(float xxsig, float yysig, float zzsig) { float pc; pres = -(xxsig+yysig+zzsig)/3.0; pc = -1000; if (pres < pc) { return 1.0; } else { return 0.0; } } Example 2: The second example switches the material if it goes through a segment. *comment units: mks Switch the 1st group to the 2nd group if the ALE element center goes through a segment of the set defined by idsegset = 1. The segment position is updated every cycle A fraction of the material is switched. This fraction depends on the distance between the segment and element centers time : 47th variable cycle : 48th variable xsld : 49th variable (x-position of the element center) ysld : 50th variable (y-position of the element center) zsld : 51th variable (z-position of the element center) xseg : 52th variable (x-position of the segment center) yseg : 53th variable (y-position of the segment center) zseg : 54th variable (z-position of the segment center) xn : 55th variable (x-component of the segment normal) yn : 56th variable (y-component of the segment normal) zn : 57th variable (z-component of the segment normal) volmat1 : 43th variable (material volume of the 1st group) volfrac1: 45th variable (volume fraction of the 1st group) segsurf : segment surface (given by 0.5*sqrt(xn*xn+yn*yn+zn*zn)) sldvol : ALE element volume (given by volmat1/volfrac1) segcharaclen: characteristic length for the segment sldcharaclen: characteristic length for the solid xseg2sld: x-component of the vector segment center to element center yseg2sld: y-component of the vector segment center to element center zseg2sld: z-component of the vector segment center to element center distnormseg2sld: Distance segment-element projected on the normal disttangseg2sld: Distance segment-element projected on the segment plane *ALE_SWITCH_MMG $# fr_mmg to_mmg idfunc idsegset idsldset ncycseg ncycsld 1 2 11 1 1 47 57 43 45 *set_multi-material_group_list 1 1 *set_multi-material_group_list 2 2 *DEFINE_FUNCTION 11 float switchmmg(float time, float cycle, float xsld, float ysld, float zsld, float xseg, float yseg, float zseg, float xn, float yn, float zn, float volmat1, float volfrac1) { float segsurf, sldvol, segcharaclen, sldcharaclen; float xseg2sld, yseg2sld, zseg2sld, distnormseg2sld; float xtangseg2sld, ytangseg2sld, ztangseg2sld, disttangseg2sld; float frac; segsurf = sqrt(xn*xn+yn*yn+zn*zn); if (segsurf != 0.0) { xn = xn/segsurf; yn = yn/segsurf; zn = zn/segsurf; } segsurf = 0.5*segsurf; sldvol = volmat1/volfrac1; segcharaclen = 0.5*sqrt(segsurf); sldcharaclen = 0.5*sldvol**(1.0/3.0); xseg2sld = xsld-xseg; yseg2sld = ysld-yseg; zseg2sld = zsld-zseg; distnormseg2sld = xseg2sld*xn+yseg2sld*yn+zseg2sld*zn; xtangseg2sld = xseg2sld-distnormseg2sld*xn; ytangseg2sld = yseg2sld-distnormseg2sld*yn; ztangseg2sld = zseg2sld-distnormseg2sld*zn; disttangseg2sld = xtangseg2sld*xtangseg2sld+ ytangseg2sld*ytangseg2sld+ ztangseg2sld*ztangseg2sld; disttangseg2sld = sqrt(disttangseg2sld); if (disttangseg2sld <= segcharaclen && distnormseg2sld <= sldcharaclen) { sldcharaclen = 2.0*sldcharaclen; frac = distnormseg2sld/sldcharaclen; frac = 0.5-frac; return frac; } else { return 0.0; } } *ALE_TANK_TEST Purpose: Control volume airbags (*AIRBAG_) only require two engineering curves to define gas inflator, i.e. 𝑚̇ (𝑡) and 𝑇̅̅̅̅̅ gas(𝑡); those two curves can be experimentally measured. However, the ALE inflator needs one additional state variable - the inlet gas velocity which is impractical to obtain. This keyword is to provide such curve through an engineering approximation. It takes two curves from the accompanying *SECTION_POINT_SOURCE as input. It assumes inflator gas under choking condition to generate velocity curve. During this process, the original curves, 𝑚̇ (𝑡) and 𝑇̅̅̅̅̅ gas(𝑡), are modified accordingly. It complements and must be used together with the*SECTION_POINT_SOURCE command. Please see *SECTION_POINT_SOURCE for additional information. Card 1 1 2 3 4 5 6 7 8 Variable MDOTLC TANKV PAMB PFINAL MACHL VELMAX AORIF Type Default I 0 I I I F F F 0.0 0.0 0.0 0.0 0.0 0.0 Card 2 1 2 3 4 5 6 7 8 Variable AMGIDG AMGIDA NUMPNT Type Default I 0 I 0 I 50 VARIABLE MDOTLC TANKV DESCRIPTION LCID for mass flow rate as a function of time. This may be obtained directly from the control-volume type input data. Volume of the tank used in a tank test from which the tank pressure is measured, and 𝑚̇ (𝑡) and 𝑇̅̅̅̅gas(𝑡) are computed from this tank pressure data. VARIABLE DESCRIPTION PAMB The pressure inside the tank before jetting (usually 1bar). PFINAL The final equilibrated pressure inside the tank from the tank test. MACHL VELMAX AORIF A limiting MACH number for the gas at the throat (MACH = 1 preferred). Maximum allowable gas velocity across the inflator orifice (not preferred). Total inflator orifice area (optional, only needed if the *SEC- TION_POINT_SOURCE card is not used). AMGIDG The ALE multi-material group ID (AMMGID) of the gas. AMGIDA The ALE multi-material group ID (AMMGID) of the air. NUMPNT The number of points NUMPNT = 0, defaults to 50 points. in 𝑚̇ (𝑡) and 𝑇̅̅̅̅gas(𝑡) curves. If Remarks: In an airbag inflator tank test, the tank pressure data is measured. This pressure is used to derive 𝑚̇ (𝑡) and to estimate 𝑇̅̅̅̅gas(𝑡), the stagnation temperature of the inflator gas. This is done by applying a lumped-parameter method to the system of conservation equations using an equation of state. Together 𝑚̇ (𝑡) and 𝑇̅̅̅̅gas(𝑡) provide enough information to model an airbag with the control volume method . However, for an ALE or Eulerian fluid- structure interaction analysis, the gas velocity, 𝑣(𝑡), and density, 𝜌(𝑡), at the inlet must be computed. But, since only 𝑚̇ (𝑡) is known, additional assumptions must be made about the inlet conditions. If 𝑣(𝑡) and 𝜌(𝑡) are calculated outside of LS-DYNA, then LS- DYNA combines them with 𝑚̇ (𝑡) and 𝑇̅̅̅̅gas(𝑡) to obtain 𝑇̅̅̅̅gas corrected(𝑡), 𝑣(𝑡) and 𝜌(𝑡) which are sufficient input for an ALE calculation. The curves 𝑣(𝑡) and 𝜌(𝑡) need not be calculated outside of LS-DYNA as LS-DYNA features a method for calculating them itself. This card, *ALE_TANK_TEST, activates this capability. Thus, with the combination of this card and the *SECTION_POINT_- SOURCE card, LS-DYNA can proceed directly from the control volume method input, 𝑚̇ (𝑡) and 𝑇̅̅̅̅gas(𝑡), to an ALE or Eulerian fluid-structure interaction analysis. The user does not have to do the conversion himself. If the *ALE_TANK_TEST card is present: 1. The definitions of the relative volume, 𝑉(𝑡), and the velocity, 𝑣(𝑡), curves in the *SECTION_POINT_SOURCE card will be ignored in favor of those computed by LS-DYNA. 2. The 𝑚̇ (𝑡)curve is read in on *ALE_TANK_TEST card. 3. The 𝑇gas(𝑡) curve (stagnation temperature), as opposed to 𝑇gas corrected(𝑡), is read in on *SECTION_POINT_SOURCE card. There is a subtle, but important, distinction between the two temperatures. 𝑇gas(𝑡) is derived directly from the tank pressure data based on a lump- parameter approach, whereas 𝑇gas corrected(𝑡) is computed from 𝑚̇ (𝑡) and 𝑇gas(𝑡) with additional isentropic and sonic flow assumptions for the maximum veloci- ty at an orifice. 𝑇gas corrected(𝑡) is most appropriately interpreted as the static temperature. These assumptions provide a necessary and physically reasonable supplement to the governing equation, 𝑚̇ (𝑡) = 𝜌(𝑡)𝑣(𝑡)𝐴 in which only𝑚̇ (𝑡) and 𝐴 are known leaving two parameters: 𝜌(𝑡), and 𝑣(𝑡) as unkown. 4. The inflator area is computed from the *SECTION_POINT_SOURCE card that has the AMMGID of the inflator gas in the *ALE_TANK_TEST card. If the *BOUNDARY_AMBIENT_EOS card is used instead of the *SECTION_POINT_- SOURCE card, then the area may be input in this *ALE_TANK_TEST card. 5. The reference density of the propellant “gas”, 𝜌0, is computed internally and automatically used for the calculation. The 𝜌0 value from the *MAT_NULL card is ignored. Example: Consider a tank test model consists of the inflator gas (PID 1) and the air inside the tank (PID 2). The following information from the control volume model is available: • 𝑚̇ (𝑡) (LCID 1 is from control volume model input). • 𝑇̅̅̅̅gas(𝑡) (LCID 2 is from control volume model input). • Volume of the tank used in the inflator tank test. • Final equilibrated pressure inside the tank. • Ambient pressure in the air. Also available are: • The nodal IDs of the nodes defining the orifice holes through which the gas flows into the tank. • The area associated with each hole (the node is assumed to be at the center of this area). • The vector associated with each hole defining the direction of flow. In the input below LCID 1 and 2 are 𝑚̇ (𝑡) and 𝑇̅̅̅̅gas(𝑡), respectively. LCID 4 and 5 will be ignored when the *ALE_TANK_TEST card is present. If it is not present, all 3 curves in the *SECTION_POINT_SOURCE card will be used. When the *SECTION_POINT_- SOURCE card is present, the element formulation is equivalent to an ELFORM = 11. $...|....1....|....2....|....3....|....4....|....5....|....6....|....7....|...8 *PART inflator gas $ PID SECID MID EOSID HGID GRAV ADPOPT TMID 1 1 1 0 0 0 0 0 *PART air inside the tank $ PID SECID MID EOSID HGID GRAV ADPOPT TMID 2 2 2 0 0 0 0 0 *SECTION_SOLID $ SECID ELFORM AET 2 11 0 *ALE_MULTI-MATERIAL_GROUP $ SID SIDTYPE 1 1 2 1 *SECTION_POINT_SOURCE $ SECID LCIDT LCIDVOLR LCIDVEL <= 3 curves in tempvolrvel.k file 1 2 4 5 $ NODEID VECTID AREA 24485 3 15.066 ... 24557 3 15.066 *ALE_TANK_TEST $ MDOTLC TANKV PAMB PFINAL MACHL VELMAX AORIF 1 6.0E7 1.0E-4 5.288E-4 1.0 0.0 $ AMGIDG AMGIDA NUMPNT 1 2 80 $...|....1....|....2....|....3....|....4....|....5....|....6....|....7....|...8 *ALE_UP_SWITCH Purpose: For the simulation of airbag inflation process, this card allows the switching from an ALE computation to a control volume (CV) or uniform pressure (UP) method at a user-defined switch time. Card 1 1 2 3 4 5 6 7 8 Variable UPID SWTIME F 1.0e+16 Type Default Remark I 0 1 Card 2 1 2 3 4 5 6 7 8 Variable FSI_ID1 FSI_ID2 FSI_ID3 FSI_ID4 FSI_ID5 FSI_ID6 FSI_ID7 FSI_ID8 Type Default I 0 I 0 I 0 I 0 I 0 I 0 I 0 I 0 Additional card for UPID = 0 (or not defined). Optional 3 1 2 3 4 5 6 7 8 Variable SID SIDTYPE MMGAIR MMGGAS Type Default I 0 I 0 I 0 I VARIABLE UPID DESCRIPTION An ID defines a corresponding *AIRBAG_HYBRID_ID card for use in an ALE-method-switching-to-CV-method simulation. The simulation starts with ALE computational method, then switches to a CV (or UP) method at some given time. EQ.0: (or blank) The code will construct an equivalent *AIRBAG_HYBRID_ID card automatically internally, (default). The 3rd optional line is then a required input. NE.0: An ID points to a corresponding *AIRBAG_HYBRID_ID card which must be defined for use after the switch. If UPID is defined, do not define the 3rd optional card. SWTIME The time at which the computation does a switch from an ALE- method-to-CV-method. FSI_ID1, …, FSI_ID8 Coupling IDs for one or more ALE fluid-structure-interaction (FSI) cards. *CONSTRAINED_LAGRANGE_IN_SOLID_ID These couplings are deleted during the 2nd, CV computational phase. SID A set ID defines the Lagrangian parts which make up the airbag. SIDTYPE Set ID type for the above SETID (following the conventions in *AIRBAG_HYBRID card). EQ.0: SID is a segment set ID (SGSID). NE.0: SID is a part set ID (PSID). MMGAIR The AMMG (ALE multi-material group) ID of surrounding air. MMGGAS The AMMG ID of inflator gas injected into the airbag. Remarks: 1. If UPID is zero or blank, optional card 3 must be defined. LSDYNA will construct an equivalent *AIRBAG_HYBRID_ID card automatically. *ALE_UP_SWITCH Consider an airbag model with a 2-phase simulation: an ALE calculation being switched to a CV method. During the CV phase, the simulation is defined by an *AIRBAG_HYBRID_ID card. $...|....1....|....2....|....3....|....4....|....5....|....6....|....7....|....8 *ALE_UP_SWITCH $ UP_ID SW_time 100000 2.0000 $ FSI_ID_1 FSI_ID_2 FSI_ID_3 FSI_ID_4 FSI_ID_5 FSI_ID_6 FSI_ID_7 FSI_ID_8 1 2 $------------------------------------------------------------------------------- *AIRBAG_HYBRID_ID $ ID 100000 $ SID SIDTYP RBID VSCA PSCA VINI MWD SPSF 2 1 0 1.0 1.0 0.0 0.0 0.0 $ 2 ATMT ATMP ATMD GC CC 293. 1.0130e-4 1.200E-9 8.3143 1. $ C23 LCC23 A23 LCA23 CP23 LCP23 AP23 LCAP23 $ OPT PVENT NGAS 4 $bac LCIDM LCIDT NOTUSED MW INITM A B C 1001 1002 0.0288691 1.0 28.98 $ FMASS $air LCIDM LCIDT NOTUSED MW INITM A B C 1600 1603 28.97E-3 0.0 26.38 8.178e-3 -1.612e-6 $ FMASS $pyroLCIDM LCIDT NOTUSED MW INITM A B C 1601 1603 43.45E-3 0.0 32.87 2.127e-2 -5.193E-6 $ FMASS $sto_LCIDM LCIDT NOTUSED MW INITM A B C 1602 1603 39.49E-3 0.0 22.41 2.865e-3 -6.995e-7 $ FMASS $...|....1....|....2....|....3....|....4....|....5....|....6....|....7....|....8 Example 2: Consider the same airbag model with the same 2-phase simulation. However, all the *AIRBAG_HYBRID_ID card definitions are extracted automatically from the ALE model. There is no need to define the *AIRBAG_HYBRID_ID card. The 3rd optional card is required. $...|....1....|....2....|....3....|....4....|....5....|....6....|....7....|....8 *ALE_UP_SWITCH $ UP_ID SW_time $ 100000 2.0000 0 2.0000 $ FSI_ID_1 FSI_ID_2 FSI_ID_3 FSI_ID_4 FSI_ID_5 FSI_ID_6 FSI_ID_7 FSI_ID_8 1 2 $ SETID SETYPE MMG_AIR MMG_GAS 2 1 2 1 $...|....1....|....2....|....3....|....4....|....5....|....6....|....7....|....8 The keyword *BOUNDARY provides a way of defining imposed motions on boundary nodes. The keyword control cards in this section are defined in alphabetical order: *BOUNDARY_ACOUSTIC_COUPLING *BOUNDARY_ACOUSTIC_IMPEDANCE *BOUNDARY_ACOUSTIC_MAPPING *BOUNDARY_ALE_MAPPING *BOUNDARY_AMBIENT *BOUNDARY_AMBIENT_EOS *BOUNDARY_CONVECTION_OPTION *BOUNDARY_COUPLED *BOUNDARY_CYCLIC *BOUNDARY_DE_NON_REFELECTING *BOUNDARY_ELEMENT_METHOD_OPTION *BOUNDARY_FLUX_OPTION *BOUNDARY_MCOL *BOUNDARY_NON_REFLECTING *BOUNDARY_NON_REFLECTING_2D *BOUNDARY_PAP *BOUNDARY_PORE_FLUID_OPTION *BOUNDARY_PRECRACK *BOUNDARY_PRESCRIBED_ACCELEROMETER_RIGID *BOUNDARY_PRESCRIBED_FINAL_GEOMETRY *BOUNDARY_PRESCRIBED_MOTION_{OPTION1}_{OPTION2} *BOUNDARY_PRESCRIBED_ORIENTATION_RIGID_OPTION *BOUNDARY_PWP_OPTION *BOUNDARY_RADIATION_OPTION *BOUNDARY_SLIDING_PLANE *BOUNDARY_SPC_{OPTION1}_{OPTION2}_{OPTION3} *BOUNDARY_SPC_SYMMETRY_PLANE_OPTION *BOUNDARY_SPH_FLOW *BOUNDARY_SPH_NON_REFLECTING *BOUNDARY_SPH_SYMMETRY_PLANE *BOUNDARY_SYMMETRY_FAILURE *BOUNDARY_TEMPERATURE_OPTION *BOUNDARY_THERMAL_BULKFLOW_{OPTION1}_{OPTION2} *BOUNDARY_THERMAL_BULKNODE *BOUNDARY_THERMAL_WELD *BOUNDARY_THERMAL_WELD_TRAJECTORY *BOUNDARY_USA_SURFACE *BOUNDARY_ACOUSTIC_COUPLING_{OPTION} There are two forms of this keyword command: 1. for coupling of surfaces with coincident nodes *BOUNDARY_ACOUSTIC_COUPLING 2. for coupling surfaces without coincident nodes *BOUNDARY_ACOUSTIC_COUPLING_MISMATCH Purpose: Define a segment set for acoustic coupling of structural element faces and acoustic volume elements (type 8 and type 14 solid elements.) If the mismatch option is not used, then this command couples either one side of a shell or solid element structure or both sides of a shell structure to acoustic elements. The segments in the segment set should define the structural surface for which coupling is intended. The nodal points of the structural segments must be coincident with the nodal points for the fluid element faces on either side of the structural segments. If fluid exists on just one side of the structural segments, and the nodes are merged, then the input data in this section is not required. The coupling will happen automatically. However, if fluid is on both sides of the structural segments, then this input data is required and the nodes should not be merged; two-sided coupling will not properly apply loads when the interface nodes are merged out. If the mismatch option is used, then this command permits the coupling of acoustic fluid volume elements with one side of a structural element when the meshes of the fluid and structural models are moderately mismatched. In this case, it is possible that most fluid and structural nodes will not be coincident. None of the fluid and structural nodes at the interface should be merged together. The segments in the segment set should define the structural surface and, following a right hand rule, the normal vector for the segments should point at the fluid volume elements with which coupling is intended. If coupling is required on both sides of a structural shell element, duplicate segments with opposite normal vectors should be defined. Every segment in the segment set must couple with the fluid volume at some integration point, but it is not necessary that all integration points on the segment couple with the fluid. The meshes do not have to be mismatched to use mismatched coupling, as long as the fluid and structural nodes are not merged. Card 1 1 2 3 4 5 6 7 8 Variable SSID Type I Default none VARIABLE DESCRIPTION SSID Segment set ID, see *SET_SEGMENT Remarks: 1. For the stability of the acoustic-structure coupling, the following condition must be satisfied: 2𝜌𝑎𝐷 𝜌𝑠𝑡𝑠 < 5 where 𝜌𝑎 is the density of the acoustic medium, 𝐷 is the total thickness of the acoustic elements adjacent to the structural element, 𝜌𝑠 is the density, and 𝑡𝑠 is the thickness of the structural shell element. If the structural element is a solid or thick shell element, then ts should be half the thickness of the element. If coupling is on both sides of the structural elements, then ts should also be half the thickness of the structural element. 2. In mismatched coupling, free fluid faces are considered for coupling with the structural segments if they are near one another and if they face each other. Faces and segments that differ in orientation by more than 45 degrees are ex- cluded. In regions of high curvature the surfaces therefore need to be more similar than when the surfaces are flat. If a fluid face couples with any struc- tural segment, then all four integration points on the fluid face must couple with some structural segment. Fluid faces may not be partially coupled. Struc- tural segments are allowed to be partially coupled. 3. The mismatched coupling process dumps two LS-DYNA files that can be imported into LS-PrePost for review of the results of the coupling process. File “bac_str_coupling.dyn” contains shell elements where structural segments have coupled with the fluid and mass elements at structural integration points with coupling. When the messag file indicates that some structural segments have partial coupling, this file can be used to check the unconnected segment integra- tion points. File “bac_flu_coupling.dyn” contains shell elements where free fluid faces have coupled with the structural segments and mass elements at free fluid face integration points with coupling. These files are only for visualiza- tion of the coupling and serve no other purpose. *BOUNDARY_ACOUSTIC_IMPEDANCE Purpose: Define a segment set to prescribe the acoustic impedance of acoustic volume element (type 8 and type 14 solid elements) faces. Card 1 1 2 3 4 5 6 7 8 Variable SSID ZEE Type I F Default none none VARIABLE DESCRIPTION Segment set ID, see *SET_SEGMENT Value of the acoustic impedance ρc SSID ZEE Remarks: 1. The effect of the boundary impedance on the acoustic cavity response is incorporated in the forcing vector. Solutions are conditionally stable, with low values of impedance relative to the impedance of the *MAT_ACOUSTIC ele- ments causing instabilities. Reducing the factor of safety on the time step ex- tends the range of applicability, however it is recommended that pressure release conditions be handled by leaving the boundary free rather than by providing a relatively low boundary acoustic impedance value. A warning is issued if the boundary impedance value is less than 25 percent of the *MAT_- ACOUSTIC impedance. A value less than 1 percent of the *MAT_ACOUSTIC impedance is considered to be an error. Special allowance is made for cases when both *LOAD_SEGMENT set pressures and the *BOUNDARY_ACOUSTIC_IMPEDANCE are defined on the same segments. In this event a nonreflecting entrant boundary condition is assumed. The pressures in the LOAD_SEGMENT_SET definition are treated as incoming incident pressure. Pressure waves within the *MAT_ACOUSTIC domain striking this boundary will exit the model. In contrast, a *LOAD_SEG- MENT_SET on *MAT_ACOUSTIC volume faces in the absence of *BOUND- ARY_ACOUSTIC_IMPEDANCE acts as a time-dependent, total pressure constraint and pressure waves within the *MAT_ACOUSTIC domain striking this boundary will be reflected back into the model. 2. *BOUNDARY_ACOUSTIC_MAPPING Purpose: Define a set of elements or segments on structure for mapping structural nodal velocity to acoustic volume boundary. Card 1 1 2 3 4 5 6 7 8 Variable SSID STYP Type I Default none I 0 VARIABLE DESCRIPTION SSID STYP Set or part ID Set type: EQ.0: part set ID, see *SET_PART, EQ.1: part ID, see *PART, EQ.2: segment set ID, see *SET_SEGMENT. Remarks: 1. If acoustic elements are not overlapping with structural elements, this keyword passes structural velocity to acoustic volume boundary, for subsequent fre- quency domain acoustic computation. *BOUNDARY_ALE_MAPPING Purpose: This card maps ALE data histories from a previous run to a region of elements. Data are read or written in a mapping file called by the prompt “map=” on the command line . To map data at the initial time (not the histories) to all the ALE domain (not just a region of elements) see *INITIAL_ALE_- MAPPING. The following transitions are allowed: 1D → 2D 1D → 3D 2D → 2D 2D → 3D 3D → 3D Card 1 Variable 1 ID 2 3 4 5 6 7 TYP AMMSID IVOLTYP BIRTH DEATH DTOUT Type I I I I F F F Default none none none none 0.0 1020 Card 2 1 2 Variable THICK RADIUS Type F F 3 X1 F 4 Y1 F 5 Z1 F 6 X2 F time step 7 Y2 F 8 INI I 0 8 Z2 F Default 0.0 0.0 0.0 0.0 0.0 0.0 0.0 0.0 Card 3 Variable 1 XO Type F 2 YO F 3 ZO F 4 5 6 7 8 VECID I Default 0.0 0.0 0.0 none VARIABLE DESCRIPTION ID TYP Part ID or part set ID or element set ID Type of “ID” : EQ.0: part set ID. EQ.1: part ID. EQ.2: shell set ID. EQ.3: solid set ID. AMMSID IVOLTYP Set ID of ALE multi-material groups defined in *SET_MULTI- MATERIAL_GROUP. See Remark 1. Type of volume containing the selected elements for the mapping. The absolute value of IVOLTYPE indicates the type of volume and the sign indicates whether the data is being read of written. Volume Type |IVOLTYP|.EQ.1: Spherical surface with thickness (THICK). |IVOLTYP|.EQ.2: Box. |IVOLTYP|.EQ.3: Cylindrical surface with thickness (THICK) |IVOLTYP|.EQ.4: All the elements defined by ID. Read/Write IVOLTYP.LT.0: data from the mapping file are read for the elements of this volume. IVOLTYP.GT.0: data from the elements of this volume are written in the mapping file. BIRTH DEATH Birth time to write or read the mapping file. If a mapping file is written, the next run reading this file will begin at time BIRTH if this parameter for this next run is not larger. Death time to write or read the mapping file. If a mapping file is written, the next run will stop to read this file at time DEATH if this parameter for this next run is not smaller. DTOUT Time interval between outputs in the mapping file. This parameter is only used to write in the mapping file. VARIABLE DESCRIPTION INI Flag to initialize all the ALE domain of the next run: EQ.0: No initialization EQ.1: Initialization. *INITIAL_ALE_MAPPING will have to be in the input deck of the next run to read the data from the mapping file. The initial time of the next run will be BIRTH. THICK Thickness for the element selection using surfaces. RADIUS Radius for abs(IVOLTYP) = 1 and abs(IVOLTYP) = 3. If abs(IVOLTYP).EQ.1: X1 Y1 Z1 X1 is the 𝑥-coordinate of the sphere center. Y1 is the 𝑦-coordinate of the sphere center. Z1 is the 𝑧-coordinate of the sphere center. X2, Y2, Z2 Ignored If abs(IVOLTYP).EQ.2: X1 Y1 Z1 X2 Y2 Z2 X1 is the 𝑥-coordinate of the box’s minimum point. Y1 is the 𝑦-coordinate of the box’s minimum point. Z1 is the 𝑧-coordinate of the box’s minimum point. X2 is the 𝑥-coordinate of the box’s maximum point. Y2 is the 𝑦-coordinate of the box’s maximum point. Z2 is the 𝑧-coordinate of the box’s maximum point. VARIABLE DESCRIPTION If abs(IVOLTYP).EQ.3: X1 Y1 Z1 X2 Y2 Z2 X1 is the 𝑥-coordinate of a point on the cylinder’s axis. Y1 is the 𝑦-coordinate of a point on the cylinder’s axis. Z1 is the 𝑧-coordinate of a point on the cylinder’s axis. X2 is the 𝑥-coordinate of a vector parallel to the cylinder’s axis. Y2 is the 𝑦-coordinate of a vector parallel to the cylinder’s axis. Z2 is the 𝑧-coordinate of a vector parallel to the cylinder’s axis. If abs(IVOLTYP).EQ.4: X1, Y1, Z1 ignored X2, Y2, Z2 ignored End if X0 Y0 Z0 Origin position in global 𝑥-direction. See Remark 2. Origin position in global 𝑦-direction. See Remark 2. Origin position in global 𝑧-direction. See Remark 2. VECID ID of the symmetric axis defined by *DEFINE_VECTOR. See Remark 3. Remarks: 1. Mapping of Multi-Material Groups. The routines of this card need to know which mesh will be initialized with the mapping data and more specifically which multi-material groups. The first 2 parameters (ID and TYP) defines the mesh and the third one (AMMSID) refer to the *SET_MULTI-MATERIAL_- GROUP_LIST card. This card will define a list of material groups in the current run. The rank in this list should match the rank of the multi-material groups from the previous run (as a reminder the ranks of multi-material groups are defined by *ALE_MULTI-MATERIAL_GROUP). For instance, if the previous model has 3 groups, the current one has 5 groups, and the following mapping is wanted: The 1st group (previous) ⇒ the 3rd group (current), The 2nd group (previous) ⇒ the 5th group (current) and, The 3rd group (previous) ⇒ the 4th group (current). Then, the *SET_MULTI-MATERIAL_GROUP_LIST card should be as follows: *SET_MULTI-MATERIAL_GROUP_LIST 300 3,5,4 2. Origin. The data can be mapped in different parts of the mesh by defining the origin of the coordinate system (X0, Y0, Z0). 3. Orientation Vector: VECID. For a mapping file created by a previous asymmetric model, the symmetric axis orientation in the current model is speci- fied by VECID. For a mapping file created by a 3D or 1D spherical model, the vector VECID is read but ignored. The definitions of X0, Y0, Z0 and VECID change in the case of the following mappings: a) plain strain 2D (ELFORM = 13 in *SECTION_ALE2D) to plain strain 2D b) plain strain 2D to 3D While, VECID still defines the y-axis in the 2D domain, the 3 first parameters in *DEFINE_VECTOR, additionally, define the location of the origin. The 3 last parameters defines a position along the y-axis. For this case when 2D data is used in a 3D calculation the point X0, Y0, Z0 together with the vector, VECID, define the plane. 4. Mapping File. To make one mapping: only the command-line argument “map=” is necessary. If IVOLTYP is positive, the mapping file will be created and ALE data histories will be written in this file. If IVOLTYP is negative the mapping file will be read and ALE data histories will be used to interpolate the ALE variables of the selected elements. This file contains the following nodal and element data: • nodal coordinates • nodal velocities • part ids • element connectivities • element centers • densities • volume fractions • stresses • plastic strains • internal energies • bulk viscosities • relative volumes 5. Successive Mappings. To make several successive mapping: the prompt “map1=” is necessary. If IVOLTYP is positive and the prompt “map1=” is in the command line, the ALE data are written to the mapping file given by “map1=”. If IVOLTYP is negative and the prompt “map=” is in the command line, ALE data are read from the mapping file given by “map=”. *BOUNDARY_AMBIENT Purpose: This command defines ALE “ambient” type element formulations (please see Remarks 1, 2 and 5). Card 1 1 2 3 4 5 6 7 8 Variable SETID MMG AMBTYP Type I I I Default none none none Optional Card. Additional optional card for AMBTYP = 4 with curves Card 3 1 2 3 4 5 6 7 8 Variable LCID1 LCID2 Type I I Default none none VARIABLE SETID DESCRIPTION The ambient element set ID for which the thermodynamic state is being defined. The element set can be *SET_SOLID for a 3D ALE model, *SET_SHELL for a 2D ALE model or *SET_BEAM for a 1D ALE model. MMG ALE multi-material group ID. AMBTYP Ambient element type: EQ.4: Pressure inflow/outflow EQ.5: Receptor for blast load DESCRIPTION A load curve ID for internal energy per unit reference volume (Please see Remark 4 and read the beginning of the EOS section for details). If *EOS_IDEAL_GAS is being used, this ID then refers to a temperature load curve ID. Load curve ID for relative volume, 𝑣𝑟 = ( 𝑣 𝑣0 Remark 3 and read the beginning of the EOS section for details). 𝜌0 𝜌 ). (Please see = VARIABLE LCID1 LCID2 Remarks: 1. The term “ambient” refers to a medium that has predetermined thermodynam- ic state throughout the simulation. All “ambient” elements will have its ther- modynamic state reset back to this predetermined state every cycle. If this state is defined via the *EOS card, then this predetermined thermodynamic state is constant throughout the simulation. If it is defined via the curves of the 2nd line for AMBTYP = 4, its thermodynamic state will vary according to these defined load curves. “Ambient” elements are sometimes also referred to as “reservoir” elements as they may be used to simulate semi-infinite region. 2. In general, a thermodynamic state of a non-reacting and no-phase-change material may be defined by 2 thermodynamic variables. By defining (a) an internal energy per unit reference volume load curve (or a temperature load curve if using *EOS_IDEAL_GAS) and (b) a relative volume load curve, the pressure as a function of time for this ambient part ID can be computed directly via the equation of state (*EOS_…). 3. A reference specific volume, 𝑣0 = 1 𝜌0 , is the inverse of a reference density, 𝜌0. The reference density is defined as the density at which the material is under a reference or nominal state. Please refer to the *EOS section for additional ex- planation on this. 4. The internal energy per unit reference volume may be defined as 𝑒ipv0 = 𝐶𝑣𝑇 𝑣0 . The specific internal energy (or internal energy per unit mass) is defined as 𝐶𝜈𝑇. 5. This card does not require AET under *SECTION_SOLID or SECTION_ALE2D or SECTION_ALE1D card *BOUNDARY_AMBIENT_EOS Purpose: This command defines the IDs of 2 load curves: (1) internal energy per unit reference volume (or temperature if using *EOS_IDEAL_GAS) and (2) relative volume. These 2 curves completely prescribe the thermodynamic state as a function of time for any ALE or Eulerian part with an “ambient” type element formulation (please see Remark 4). Card 1 1 2 3 4 5 6 7 8 Variable PID LCID1 LCID2 Type I I I Default none none none VARIABLE DESCRIPTION The ambient Part ID for which the thermodynamic state is being defined. Load curve ID (*DEFINE_CURVE or *DEFINE_CURVE_FUNC- TION) for internal energy per unit reference volume (please read the beginning of the EOS section for details). If *EOS_IDEAL_- GAS is being used, this ID then refers to a temperature load curve ID. Load curve ID (*DEFINE_CURVE or *DEFINE_CURVE_FUNC- 𝜌0 TION) for relative volume, 𝑣𝑟 = ( 𝑣 𝜌 ). (Please read the = 𝑣0 beginning of the EOS section for details). PID LCID1 LCID2 Remarks: 1. The term “ambient” refers to a medium that has predetermined thermodynam- ic state throughout the simulation. All “ambient” parts/elements will have its thermodynamic state reset back to this predetermined state every cycle. If this state is defined via the *EOS card, then this predetermined thermodynamic state is constant throughout the simulation. If it is defined via this card, *BOUNDARY_AMBIENT_EOS, then its thermodynamic state will vary accord- ing to these defined load curves. “Ambient” part is sometimes also referred to as “reservoir” part as it may be used to simulate semi-infinite region. 2. In general, a thermodynamic state of a non-reacting and no-phase-change material may be defined by 2 thermodynamic variables. By defining (a) an internal energy per unit reference volume load curve (or a temperature load curve if using *EOS_IDEAL_GAS) and (b) a relative volume load curve, the pressure as a function of time for this ambient part ID can be computed directly via the equation of state (*EOS_…). 3. A reference specific volume, 𝑣0 = 1 𝜌0 , is the inverse of a reference density, 𝜌0. The reference density is defined as the density at which the material is under a reference or nominal state. Please refer to the *EOS section for additional ex- planation on this. 4. The internal energy per unit reference volume may be defined as 𝑒ipv0 = 𝐶𝑣𝑇 𝑣0 . The specific internal energy (or internal energy per unit mass) is defined as 𝐶𝜈𝑇. 5. This card is only to be used with “ambient” element type as defined by the parameters under the *SECTION_SOLID card: a) ELFORM = 7, or b) ELFORM = 11 and AET = 4, or c) ELFORM = 12 and AET = 4. Example: Consider an ambient ALE part ID 1 which has its internal energy per unit reference volume in a load curve ID 2 and relative volume load curve ID 3: $...|....1....|....2....|....3....|....4....|....5....|....6....|....7....|...8 *BOUNDARY_AMBIENT_EOS $ PID e/T_LCID rvol_LCID 1 2 3 $...|....1....|....2....|....3....|....4....|....5....|....6....|....7....|...8 *BOUNDARY_CONVECTION_OPTION Available options include: SEGMENT SET Purpose: Apply a convection boundary condition on a SEGMENT or SEGMENT_SET for a thermal analysis. Two cards are defined for each option. Card 1 for SET keyword option. Card 1 1 2 3 4 5 6 7 8 Variable SSID Type I Default none Card 1 for SEGMENT keyword option. Card 1 Variable 1 N1 Type I 2 N2 I 3 N3 I 4 N4 I Default none none none none 5 6 7 8 Card 2 1 2 3 4 5 6 7 8 Variable HLCID HMULT TLCID TMULT LOC Type I F I F Default none 0. none 0. I VARIABLE DESCRIPTION SSID Segment set ID, see *SET_SEGMENT. N1, N2, …. Node ID’s defining segment. HLCID Convection heat transfer coefficient, ℎ. This parameter can reference a load curve ID or a function ID . When the reference is to a curve, HLCID has the following interpretation: GT.0: ℎ is given as a function of time, 𝑡. The curve consists of (𝑡, ℎ(𝑡)) data pairs. EQ.0: ℎ is a constant defined by the value HMULT. LT.0: ℎ is given as a function of temperature, 𝑇𝑓𝑖𝑙𝑚. The curve consists of (𝑇𝑓𝑖𝑙𝑚, ℎ) data pairs. Enter |HLCID| on the DEFINE_CURVE keyword. HMULT Convection heat transfer coefficient, ℎ, curve multiplier. TLCID Environment temperature, 𝑇∞. This parameter can reference a load curve ID or a function ID . When the reference is to a curve, TLCID has the following interpretation: GT.0: 𝑇∞ is defined by a curve indexed by time consisting of (𝑡, 𝑇∞(𝑡)) data pairs. EQ.0: 𝑇∞ is a constant defined by the value TMULT. TMULT Environment temperature, 𝑇∞, curve multiplier. LOC For a thick thermal shell, the convection will be applied to the surface identified by LOC. See parameter, THSHEL, on the *CONTROL_SHELL keyword. EQ.-1: lower surface of thermal shell element EQ.0: middle surface of thermal shell element EQ.1: upper surface of thermal shell element Remarks: 1. A convection boundary condition is calculated using 𝑞 ̇′′ = ℎ(𝑇surface − 𝑇∞) where h is the heat transfer coefficient, and 𝑇surface − 𝑇∞ is a temperature poten- tial. If h is a function of temperature, h is evaluated at the average or “film” temperature defined by 𝑇𝑓𝑖𝑙𝑚 = (𝑇surface + 𝑇∞)/2.. 2. If HLCID references a DEFINE_FUNCTION, the following function arguments are allowed 𝑓 (𝑥, 𝑦, 𝑧, 𝑣𝑥, 𝑣𝑦, 𝑣𝑍, 𝑇, 𝑇∞, 𝑡) where: 𝑥, 𝑦, 𝑧 = segment centroid coordinates 𝑣𝑥, 𝑣𝑦, 𝑣𝑧 = segment centroid velocity component 𝑇 = segment centroid temperature 𝑇∞ = environment temperature, T∞ 𝑡 = solution time 3. If TLCID references a DEFINE_FUNCTION, the following function arguments are allowed 𝑓 (𝑥, 𝑦, 𝑧, 𝑣𝑥, 𝑣𝑦, 𝑣𝑧, 𝑡) where: 𝑥, 𝑦, 𝑧 = segment centroid coordinates 𝑣𝑥, 𝑣𝑦, 𝑣𝑧 = segment centroid velocity components 𝑡 = solution time *BOUNDARY Purpose: Define a boundary that is coupled with an external program. Two cards are required for each coupled boundary Card 1 Variable 1 ID Type I 2 3 4 5 6 7 8 TITLE A70 Card 2 1 2 3 4 5 6 7 8 Variable SET TYPE PROG Type I I I Default none none none VARIABLE DESCRIPTION ID ID for this coupled boundary TITLE Descriptive name for this boundary SET TYPE Node set ID Coupling type: EQ.1: node set with force feedback EQ.2: node set for multiscale spotwelds PROG Program to couple to EQ.1: MPP-DYNA Remarks: This option is only available in the MPP version, and allows for loose coupling with other MPI programs using a “multiple program” execution method. Currently it is only useful when linking with MPP-DYNA for the modeling of multiscale spotwelds (type = 2, prog = 1). See *INCLUDE_MULTISCALE_SPOTWELD for information about using this capability. *BOUNDARY OPTION allows an optional ID to be given that applies each cyclic definition ID Purpose: Define nodes in boundary planes for cyclic symmetry. These boundary conditions can be used to model a segment of an object that has rotational symmetry such as an impeller, i.e., Figure 5-1. The segment boundary, denoted as a side 1 and side 2, may be curved or planar. In this section, a paired list of points are defined on the sides that are to be joined. ID Card. Additional card for ID keyword option. 2 3 4 5 6 7 8 ID Variable 1 ID Type I Card 1 Variable 1 XC Type F 2 YC F 3 ZC F HEADING A70 4 5 6 7 8 NSID1 NSID2 IGLOBAL ISORT I I I 0 I 0 Default none none none none none VARIABLE DESCRIPTION XC YC ZC x-component axis vector of axis of rotation y-component axis vector of axis of rotation z-component axis vector of axis of rotation NSID1 Node set ID for first boundary (side 1, see Figure 5-1). Conformable Interface Side 1 e 2 Sid Segment Figure 5-1. With axi-symmetric cyclic symmetry, only one segment is modeled. VARIABLE NSID2 DESCRIPTION Node set ID for second boundary (side 2, see Figure 5-1). Each node in this set is constrained to its corresponding node in the first node set. Node sets NSID1 and NSID2 must contain the same number of nodal points. The shape of the two surfaces formed by the two node sets need not be planar but the shapes should match. IGLOBAL Flag for repeating symmetry: EQ.0: Axi-symmetric cyclic symmetry (default) EQ.1: Repeating symmetry in planes normal to global X EQ.2: Repeating symmetry in planes normal to global Y EQ.3: Repeating symmetry in planes normal to global Z ISORT Set to 1 for automatic sorting of nodes in node sets. See Remark 2. Remarks: 1. Each node set should generally be boundaries of the model. 2. Prior to version 970, it was assumed that the nodes are correctly ordered within each set, i.e. the nth node in NSID1 is equivalent to the nth node in NSID2. In version 970 and later versions, if the ISORT flag is active, the nodes in NSID2 are automatically sorted to achieve equivalence, so the nodes can be picked by the quickest available method. However, for axi-symmetric cyclic symmetry (IGLOBAL = 0), it is assumed that the axis passes through the origin, i.e., only globally defined axes of rotation are possible. *BOUNDARY_DE_NON_REFLECTING Purpose: Define a non-reflecting boundary for discrete element. Card 1 1 2 3 4 5 6 7 8 Variable NSID Type I Default none Remarks 1, 2 VARIABLE DESCRIPTION NSID Node set ID, see *SET_SEGMENT. Remarks: 1. Non-reflecting boundaries are used on the exterior boundaries of an analysis model of an infinite domain, such as a half-space to prevent artificial stress wave reflections generated at the model boundaries form reentering the model and contaminating the results. Available options include: SEGMENT SET *BOUNDARY Purpose: Apply a flux boundary condition on a SEGMENT or SEGMENT_SET for a thermal analysis. Two or more cards are defined for each option. History variables can be associated with the boundary condition which will invoke a call to a user defined boundary flux subroutine for computing the flux. Card 1 for SET option. Card 1 1 2 3 4 5 6 7 8 Variable SSID Type I Default none Card 1 for SEGMENT option. Card 1 Variable 1 N1 Type I 2 N2 I 3 N3 I 4 N4 I Default none none none none 5 6 7 Card 2 1 2 3 4 5 6 7 8 Variable LCID MLC1 MLC2 MLC3 MLC4 LOC NHISV Type I F Default none 0. F 0. F 0. F 0. I 0 I 0 Define as many cards as necessary to initialize NHISV history variables. Card 3 1 2 3 4 5 6 7 8 Variable HISV1 HISV2 HISV3 HISV4 HISV5 HISV6 HISV7 HISV8 Type F Default 0. F 0. F 0. F 0. F 0. F 0. F 0. F 0. VARIABLE DESCRIPTION SSID Segment set ID, see *SET_SEGMENT N1, N2, … Node IDs that define the segment VARIABLE LCID DESCRIPTION This parameter can reference a load curve ID or a function ID for heat flux. When the reference is to a curve, LCID has the following interpretation: GT.0: the flux is defined by a curve consisting of (time, flux) data pairs using the DEFINE_CURVE keyword. The flux value applied to the nodal points is the curve value mul- tiplied by the values MLC1, MLC2, MLC3, and MLC4, respectively. EQ.0: a constant flux is applied to each node defined by the values MLC1, MLC2, MLC3, and MLC4, respectively. LT.0: the flux is defined by a curve consisting of (temperature, flux) data pairs using the DEFINE_- CURVE keyword. The flux value applied to the nodal points is the curve value multiplied by the values MLC1, MLC2, MLC3, and MLC4. Enter |-LCID| on the DE- FINE_CURVE keyword. MLC1 MLC2 MLC3 MLC4 LOC Curve multiplier at node N1. Curve multiplier at node N2. Curve multiplier at node N3. Curve multiplier at node N4. For a thick thermal shell, the flux will be applied to the surface identified by LOC. See parameter, THSHEL, on the *CON- TROL_SHELL keyword. EQ.-1: lower surface of thermal shell element EQ.0: middle surface of thermal shell element EQ.1: upper surface of thermal shell element NHISV Number of history variables associated with the flux definition: GT.0: A user defined subroutine will be called to compute the flux. See Remark 1. HISV1 HISV2 Initial value of history variable 1 Initial value of history variable 2 VARIABLE DESCRIPTION ⋮ ⋮ HISVn Initial value of history variable n, where n = NHISV Remarks: 1. The segment normal has no bearing on the flux. A positive flux transfers energy into the volume; a negative flux transfers energy out of the volume. 2. Flux can be defined by: a) When LCID = 0, a constant flux is applied to each node defined by the values MLC1, MLC2, MLC3, and MLC4, respectively. b) When LCID > 0, the flux is defined by a curve consisting of (time, flux) data pairs using the DEFINE_CURVE keyword. The flux value applied to the nodal points is the curve value multiplied by the values MLC1, MLC2, MLC3, and MLC4, respectively. c) When LCID < 0, the flux is defined by a curve consisting of (temperature, flux) data pairs using the DEFINE_CURVE keyword. The flux value applied to the nodal points is the curve value multiplied by the values MLC1, MLC2, MLC3, and MLC4. Enter |LCID| on the DEFINE_- CURVE keyword. d) When NHSIV > 0, the user subroutine subroutine usrflux(fl, flp, ...) will be called to compute the heat flux (fl). For more details see Appen- dix S. e) If LCID references a DEFINE_FUNCTION, the following function argu- ments are allowed 𝑓 (𝑥, 𝑦, 𝑧, 𝑣𝑥, 𝑣𝑦, 𝑣𝑧, 𝑇, 𝑇∞, 𝑡) where: 𝑥, 𝑦, 𝑧 = segment centroid coordinates 𝑣𝑥, 𝑣𝑦, 𝑣𝑧 = segment centroid velocity components 𝑇 = segment centroid temperature 𝑇∞ = environment temperature, T∞ 𝑡 = solution time 3. This keyword is supported in the SPH elements to define the flux boundary conditions for a thermal or coupled thermal/structural analysis. The values 𝑛1, 𝑛2, 𝑛3, 𝑛4 from the SPH particles or segments are used to define the flux seg- ments. *BOUNDARY_MCOL Purpose: Define parameters for MCOL coupling. The MCOL Program is a rigid body mechanics program for modeling the dynamics of ships. See Remark 1 for more information. Card 1 1 2 3 4 5 6 7 8 Variable NMCOL MXSTEP ETMCOL TSUBC PRTMCOL Type Default I 2 I F F F none 0.0 0.0 none Remarks 2 Ship Card. Include NMCOL cards, one for each ship. Card 2 1 2 3 4 5 6 7 8 Variable RBMCOL MCOLFILE Type I Default A60 none VARIABLE DESCRIPTION NMCOL Number of ships in MCOL coupling. MXSTEP Maximum of time step in MCOL calculation. If the number of MCOL time steps exceeds MXSTEP, then LS-DYNA will terminate. ETMCOL Uncoupling termination time, see Remark 2 below. EQ.0.0: set to LS-DYNA termination time TSUBC Time interval for MCOL subcycling. EQ.0.0: no subcycling VARIABLE DESCRIPTION PRTMCOL Time interval for output of MCOL rigid body data. RBMCOL LS-DYNA rigid body material assignment for the ship. MCOLFILE Filename containing MCOL input parameters for the ship. Remarks: 1. The basis for MCOL is a convolution integral approach for simulating the equations of motion. A mass and inertia tensor are required as input for each ship. The masses are then augmented to include the effects of the mass of the surrounding water. A separate program determines the various terms of the damping/buoyancy force formulas which are also input to MCOL. The cou- pling is accomplished in a simple manner: at each time step LS-DYNA com- putes the resultant forces and moments on the MCOL rigid bodies and passes them to MCOL. MCOL then updates the positions of the ships and returns the new rigid body locations to LS-DYNA. A more detailed theoretical and practi- cal description of MCOL can be found in a separate report (to appear). 2. After the end of the LS-DYNA/MCOL calculation, the analysis can be pursued using MCOL alone. ETMCOL is the termination time for this analysis. If ETMCOL is lower than the LS-DYNA termination time, the uncoupled analysis will not be activated. 3. The MCOL output is set to the files mcolout (ship position) and mcolenergy (energy breakdown). In LS-PrePost, mcolout can be plotted through the rigid body time history option and MCOLENERGY *BOUNDARY_NON_REFLECTING Purpose: Define a non-reflecting boundary. This option applies to continuum domains modeled with solid elements. For geomechanical problems this option is important for limiting the spatial extent of the finite element mesh and thus the number of solid elements. 4 5 6 7 8 Card 1 1 Variable SSID Type I 2 AD F 3 AS F Default none 0.0 0.0 Remarks 1, 2 3 3 VARIABLE DESCRIPTION SSID AD Segment set ID, see *SET_SEGMENT. Default activation flag for dilatational waves. EQ.0.0: on NE.0.0: off AS Default activation flag for shear waves. EQ.0.0: on NE.0.0: off Remarks: 1. Non-reflecting boundaries defined with this keyword are only used with three- dimensional solid elements. Boundaries are defined as a collection of segments, and segments are equivalent to element faces on the boundary. Segments are defined by listing the corner nodes in either a clockwise or counterclockwise order. 2. Non-reflecting boundaries are used on the exterior boundaries of an analysis model of an infinite domain, such as a half-space to prevent artificial stress wave reflections generated at the model boundaries form reentering the model and contaminating the results. Internally, LS-DYNA computes an impedance matching function for all non-reflecting boundary segments based on an as- sumption of linear material behavior. Thus, the finite element mesh should be constructed so that all significant nonlinear behavior is contained within the discrete analysis model. 3. With the two optional switches, the influence of reflecting waves can be studied. 4. During the dynamic relaxation phase (optional), nodes on non-reflecting segments are constrained in the normal direction. Nodal forces associated with these constraints are then applied as external loads and held constant in the transient phase while the constraints are replaced with the impedance matching functions. In this manner, soil can be quasi-statically prestressed during the dynamic relaxation phase and dynamic loads (with non-reflecting boundaries) subsequently applied in the transient phase. 5. In explicit analyses this command has the side effect of reducing the default value for the time step scale factor from 0.9 to 0.667. A nonzero value of TSS- FAC in *CONTROL_TIMESTEP will override that default. *BOUNDARY_NON_REFLECTING_2D Purpose: Define a non-reflecting boundary. This option applies to continuum domains modeled with two-dimensional solid elements in the xy plane. For geomechanical problems, this option is important for limiting the size of the models. Card 1 1 2 3 4 5 6 7 8 Variable NSID Type I Default none Remarks 1, 2 VARIABLE DESCRIPTION NSID Node set ID, see *SET_NODE. See Figure 5-2. Remarks: 1. Non-reflecting boundaries defined with this keyword are only used with two- dimensional solid elements in either plane strain or axisymmetric geometries. Boundaries are defined as a sequential string of nodes moving counterclock- wise around the boundary. 2. Non-reflecting boundaries are used on the exterior boundaries of an analysis model of an infinite domain, such as a half-space to prevent artificial stress wave reflections generated at the model boundaries from reentering the model and contaminating the results. Internally, LS-DYNA computes an impedance matching function for all non-reflecting boundary segments based on an as- sumption of linear material behavior. Thus, the finite element mesh should be constructed so that all significant nonlinear behavior in contained within the discrete analysis model. Define the nodes k, k+1, k+2, ..., k+n while moving counterclockwise around the boundary. k+2 k+1 k+n Figure 5-2. When defining a transmitting boundary in 2D define the node numbers in the node set in consecutive order while moving counterclockwise around the boundary. *BOUNDARY_PAP Purpose: Define pressure boundary conditions for pore air flow calculation, e.g. at structure surface exposed to atmospheric pressure. Card 1 1 2 3 4 5 6 7 8 Variable SEGID LCID CMULT CVMASS BLOCK TBIRTH TDEATH CVRPER Type I F F F F Default none none none none 0.0 0.0 1.e20 1.0 Remark 1, 2 3 VARIABLE DESCRIPTION SEGID Segment set ID LCID Load curve giving pore air pressure vs. time. EQ.0: constant pressure assumed equal to CMULT CMULT Factor on curve or constant pressure head if LCID = 0 CVMASS Initial mass of a control volume next to the segment set SETID BLOCK Contact blockage effect, EQ.0: When all segments in SEGID are subject to the pressure defined by LCID and CMULT; EQ.1: When only elements in SEGID not involved in contact are subject to the pressure defined by LCID and CMULT. TBIRTH Time at which boundary condition becomes active TDEATH Time at which boundary condition becomes inactive CVRPER Permeability factor of cover material, where cover refers to a shell layer coating the surface of the solid. Default value is 1.0 when it is not defined. See Remark 3 below. 0.0 ≤ CVRPER ≤ 1.0 Control Volume SEGID Segment ID for the part of the boundary through which air flows to and from the control volume. Sample Figure 5-3. Air flows between the control volume and the sample. CVMASS specifies the control volume’s initial mass, and CVMULT sets the initial pressure. Remarks: 1. All structure surfaces subject to specified pressure have to be defined. 2. A non-zero CVMASS, together with a non-zero CMULT and an un-defined LCID, can be used to simulate air mass transfer between a control volume and a test specimen containing pore air. The control volume is assumed to have a fixed volume, and have initial pressure of CMULT and initial mass of CVMASS. Air mass transfer happens between control volume and its neighbor- ing specimen. Such mass transfer results in pressure change in control volume and test specimen. 3. CVRPER allows users to model the porosity properties of the cover material. If SEGID is covered by a material of very low permeability (e.g., coated fabric), it is appropriate to set CVRPER = 0. In this case, Pc, the pressure calculated as- suming no boundary condition, is applied to SEGID. If SEGID is not covered by any material, it is appropriate to set CVRPER = 1, the default value. In this case, the applied pressure becomes Pb, the boundary pressure determined by CMULT and LCID. *BOUNDARY_PORE_FLUID_OPTION Available options include: PART SET Purpose: Define parts that contain pore fluid. Defaults are given on *CONTROL_- PORE_FLUID. Card 1 1 2 3 4 5 6 7 8 Variable P(S)ID WTABLE PF_RHO ATYPE PF_BULK ACURVE WTCUR SUCLIM Type I Default none F * F * I * F * I 0 I 0 F 0. * Defaults are taken from *CONTROL_PORE_FLUID VARIABLE PID, PSID DESCRIPTION Part ID (PID) or Part set ID, see *PART and *SET_PART. All elements within the part must lie below the water table. WTABLE Z-coordinate at which pore pressure = 0 (water table) PF_RHO Density of pore water in soil skeleton: EQ.0: Default density specified on *CONTROL_PORE_FLUID card is used. ATYPE Analysis type for Parts: EQ.0: Default to value specified on *CONTROL_PORE_FLUID EQ.1: Undrained analysis EQ.2: Drained analysis EQ.3: Time dependent consolidation (coupled) EQ.4: Consolidate to steady state (uncoupled) EQ.5: Drained in dynamic relaxation, undrained in transient VARIABLE DESCRIPTION PF_BULK Bulk modulus of pore fluid: EQ.0: Default to value specified on *CONTROL_PORE_FLUID ACURVE Curve of analysis type vs time WTCUR Curve of water table (z-coordinate) vs time SUCLIM Suction limit (defined in head, i.e. length units). Must not be negative. See remarks. Remarks: This card must be present for all parts having pore water. The density on this card is used only to calculate pressure head. To ensure the correct gravity loading, the density of the soil material should be increased to include the mass associated with the pore water. The y-axis values of the curve of analysis type vs time can only be 1, 2 or 3. During dynamic relaxation, the analysis type will be taken from the first value on the curve The default for SUCLIM is zero, meaning that the pore fluid cannot generate suction. To allow unlimited suction, set this parameter to a large positive number. *BOUNDARY_PRECRACK Purpose: Define pre-cracks in XFEM shell formulations 52 or 54 for purposes of fracture analysis. 4 5 6 7 8 Card 1 1 2 Variable PID CTYPE Type I Default I 1 3 NP I Precrack Point Cards. Include NP cards, one for each point in the pre-crack. 4 5 6 7 8 1 X F 2 Y F 3 Z F Card 2 Variable Type Default VARIABLE DESCRIPTION PID Part ID where the pre-crack is located CTYPE Type of pre-crack: EQ.1: straight line NP Number of points defining the pre-crack X, Y, Z Coordinates of the points defining the pre-crack *BOUNDARY_PRESCRIBED_ACCELEROMETER_RIGID Purpose: Prescribe the motion of a rigid body based on experimental data obtained from accelerometers affixed to the rigid body. Note: This feature is available starting with LS-DYNA 971R3. Card 1 1 2 3 4 5 6 7 8 Variable PID SOLV Type I Default none I 1 Accelerometer Cards. Define one card for each accelerometer affixed to the rigid body. Input is terminated when a “*” card is found. A minimum of three accelerometers are required . Card 2 1 2 3 4 5 6 7 8 Variable NID CID LCIDX LCIDY LCIDZ Type I I I I I Default none none none none none VARIABLE DESCRIPTION PID Part ID for rigid body whose motion is prescribed. SOLV Solver type: EQ.1: Gaussian elimination (default), EQ.2: linear regression NID CID Node ID corresponding to the location of the accelerometer. the Coordinate system accelerometer’s *DEFINE_COORDINATE_- NODES). All nodes must reside on the same part. Set FLAG = 1. the orientation of ID describing local axes (see VARIABLE DESCRIPTION Load curve ID containing the local x-acceleration time history from the accelerometer. Load curve ID containing the local y-acceleration time history from the accelerometer. Load curve ID containing the local z-acceleration time history from the accelerometer. LCIDX LCIDY LCIDZ Remarks: 1. Acceleration time histories from a minimum of three accelerometers each providing output from three channels are required. Load curves must have the same number of points and data must be uniformly spaced. 2. Local axes of the accelerometers must be orthogonal. *BOUNDARY_PRESCRIBED_FINAL_GEOMETRY The final displaced geometry for a subset of nodal points is defined. The nodes of this subset are displaced from their initial positions specified in the *NODE input to the final geometry along a straight line trajectory. A load curve defines a scale factor as a function of time that is bounded between zero and unity corresponding to the initial and final geometry, respectively. A unique load curve can be specified for each node, or a default load curve can apply to all nodes. The external work generated by the displacement field is included in the energy ratio calculation for the glstat file. Card 1 1 2 3 4 5 6 7 8 Variable BPFGID LCIDF DEATHD Type Default I 0 I 0 F infinity Node Cards. The next “*” keyword card terminates this input. Card 2 1 2 3 4 5 6 7 8 9 10 Variable NID Type I X F Default none 0. Y F 0. Z F 0. LCID DEATH I F LCIDF infinity VARIABLE DESCRIPTION BPFGID ID for this set of imposed boundary conditions LCIDF Default load curve ID. This curve varies between zero and unity. DEATHD Default death time. At this time the prescribed motion is inactive and the nodal point is allowed to move freely. NID Node ID for which the final position is defined. Nodes defined in this section must also appear under the *NODE input. X x-coordinate of final geometry VARIABLE DESCRIPTION Y Z y-coordinate of final geometry z-coordinate of final geometry LCID Load curve ID. If zero the default curve ID, LCIDF, is used. DEATH Death time. If zero the default value, DEATHD, is used. *BOUNDARY_PRESCRIBED_MOTION_OPTION1_{OPTION2} Available options for OPTION1 include: NODE SET SET_BOX SET_SEGMENT RIGID RIGID_LOCAL SET_LINE OPTION2 allows an optional ID to be given that applies either to the single node, node set or a rigid body. ID If a heading is defined with the ID, then the ID with the heading will be written at the beginning of the ASCII file, bndout. Purpose: Define an imposed nodal motion (velocity, acceleration, or displacement) on a node or a set of nodes. Also velocities and displacements can be imposed on rigid bodies. If the local option is active the motion is prescribed with respect to the local coordinate system for the rigid body . Translational nodal velocity and acceleration specifications for rigid body nodes are allowed and are applied as described at the end of this section. For nodes on rigid bodies use the NODE option. Do not use the NODE option in r-adaptive problems since the node ID's may change during the adaptive step. The SET_LINE option allows a node set to be generated including existing nodes and new nodes created from h-adaptive mesh refinement along the straight line connecting two specified nodes to be included in prescribed boundary conditions. HEADING A70 5 SF F *BOUNDARY *BOUNDARY_PRESCRIBED_MOTION ID Card. Additional card for ID keyword option. 2 3 4 5 6 7 8 ID Variable 1 ID Type I Card 1 1 2 3 4 Variable typeID DOF VAD LCID Type I I Default none none I 0 I none 1. 6 7 8 VID DEATH BIRTH I 0 F F 1028 0.0 For the SET_BOX keyword option, define the following additional card. Card 2 1 2 3 4 5 6 7 8 Variable BOXID TOFFSET LCBCHK Type I Default none I 0 I 0 Additional card that is expected if DOF = 9, 10, 11 or VAD = 4 on the first card; otherwise skip this card. Card 3 1 2 3 4 5 6 7 8 Variable OFFSET1 OFFSET2 MRB NODE1 NODE2 Type F Default 0. F 0. I 0 I 0 I For the SET_LINE keyword option, define the following additional card. Card 2 1 2 3 4 5 6 7 8 Variable NBEG NEND Type I I Default none none VARIABLE DESCRIPTION ID Optional PRESCRIBED MOTION set ID to which this node, node set, segment set or rigid body belongs. This ID does not need to be unique. HEADING An optional descriptor for the given ID that will be written into the d3hsp file and the bndout file. typeID Node ID (NID in *NODE), nodal set ID (SID in *SET_NODE), segment set ID (SID in *SET_SEGMENT, see DOF = 12) or part ID (PID in *PART) for a rigid body. DOF Applicable degrees-of-freedom: EQ.1: EQ.2: EQ.3: EQ.4: EQ.-4: EQ.5: EQ.6: EQ.7: EQ.8: 𝑥-translational degree-of-freedom, 𝑦-translational degree-of-freedom, 𝑧-translational degree-of-freedom, translational motion in direction given by the VID. Movement on plane normal to the vector is permitted. translational motion in direction given by the VID. Movement on plane normal to the vector is not permit- ted. This option does not apply to rigid bodies. 𝑥-rotational degree-of-freedom, 𝑦-rotational degree-of-freedom, 𝑧-rotational degree-of-freedom, rotational motion about a vector parallel to vector VID. Rotation about the normal axes is permitted. EQ.-8: rotational motion about a vector parallel to vector VID. Rotation about the normal axes is not permitted. This VARIABLE DESCRIPTION option does not apply to rigid bodies. EQ.9: 𝑦/𝑧 degrees-of-freedom for node rotating about the 𝑥- axis at location (OFFSET1, OFFSET2) in the 𝑦𝑧-plane, point (𝑦, 𝑧). Radial motion is NOT permitted. Not ap- plicable to rigid bodies. EQ.-9: 𝑦/𝑧 degrees-of-freedom for node rotating about the 𝑥- axis at location (OFFSET1, OFFSET2) in the 𝑦𝑧-plane, point (𝑦, 𝑧). Radial motion is permitted. Not applica- ble to rigid bodies. EQ.10: 𝑧/𝑥 degrees-of-freedom for node rotating about the 𝑦- axis at location (OFFSET1, OFFSET2) in the 𝑧𝑥-plane, point (𝑧, 𝑥). Radial motion is NOT permitted. Not ap- plicable to rigid bodies. EQ.-10: 𝑧/𝑥 degrees-of-freedom for node rotating about the 𝑦- axis at location (OFFSET1, OFFSET2) in the 𝑧𝑥-plane, point (𝑧, 𝑥). Radial motion is permitted. Not applica- ble to rigid bodies. EQ.11: 𝑥/𝑦 degrees-of-freedom for node rotating about the z- axis at location (OFFSET1, OFFSET2) in the 𝑥𝑦-plane, point (𝑥, 𝑦). Radial motion is NOT permitted. Not ap- plicable to rigid bodies. EQ.-11: 𝑥/𝑦 degrees-of-freedom for node rotating about the 𝑧- axis at location (OFFSET1, OFFSET2) in the 𝑥𝑦-plane, point (𝑥, 𝑦). Radial motion is permitted. Not applica- ble to rigid bodies. EQ.12: translational motion in direction given by the normals to the segments defined by the set typeID. VAD Velocity/Acceleration/Displacement flag: EQ.0: velocity (rigid bodies and nodes), EQ.1: acceleration (rigid bodies and nodes), EQ.2: displacement (rigid bodies and nodes). EQ.3: velocity versus displacement (rigid bodies only) EQ.4: relative displacement (rigid bodies only) VARIABLE LCID DESCRIPTION Curve ID or function ID to describe motion value versus time, see *DEFINE_CURVE, *DE- FINE_FUNCTION. If LCID refers to *DEFINE_FUNCTION, the function can have only time as an argument, e.g., 𝑓 (𝑡) = 10.0 × 𝑡. See BIRTH below. *DEFINE_CURVE_FUNCTION, or SF VID Load curve scale factor. (default = 1.0) Vector ID for DOF values of 4 or 8, see *DEFINE_VECTOR. The direction of this vector is not updated with time. DEATH Time imposed motion/constraint is removed: EQ.0.0: default set to 1028 BIRTH BOXID LCBCHK Time that the imposed motion/constraint is activated. The prescribed motion begins acting at time = BIRTH but from the zero abscissa value of the curve or function (*DEFINE_FUNC- TION). In other words, the abscissae are shifted by an amount BIRTH, i.e., it has the same effect as setting OFFA = BIRTH in *DEFINE_CURVE. Warning: BIRTH is ignored if the LCID is defined as a function, i.e., *DEFINE_CURVE_FUNCTION. A box ID defining a box region in space in which the constraint is activated. Only the nodes falling inside the box will be applied the prescribed motion. If LCBCHK is not defined, the box volume is reevaluated every time step to determine the nodes for which the prescribed motion is active. This reevaluation of the volume is referred to as a “box-check”. Optional load curve allowing more flexible and efficient use of SET_BOX option. Instead of performing box-check at every time step, discrete box-check times could be given as 𝑥-values of LCBCHK. LCBCHK’s 𝑦-values specify corresponding death times. For example, a curve with points (20, 30) and (50, 70) will result in two box checks. The first will occur at 20, and the prescribed motion will be active from 20 to 30. The second will occur at 50, and the prescribed motion will be active from 50 to 70. A 𝑦-value of “0” means the prescribed motion will stay active until next box-check. For example, an additional 3rd point of (90, 0) will lead to another box-check at 90, and the prescribed motion will be active from 90 until the end of the simulation. VARIABLE DESCRIPTION TOFFSET Time offset flag for the SET_BOX option: EQ.1: the time value of the load curve, LCID, will be offset by the time when the node enters the box, EQ.0: no time offset is applied to LCID OFFSET1 Offset for DOF types 9-11 (𝑦, 𝑧, 𝑥 direction) OFFSET2 Offset for DOF types 9-11 (𝑧, 𝑥, 𝑦 direction) MRB Master rigid body for measuring the relative displacement. NODE1 Optional orientation node, n1, for relative displacement NODE2 Optional orientation node, n2, for relative displacement Node ID of a starting node. Node ID of an ending node. All existing nodes and new nodes generated by h-adaptive mesh refinement along the straight line connecting NBEG and NEND will be included in the prescribed boundary motions. NBEG NEND Remarks: When DOF = 5, 6, 7, or 8, nodal rotational degrees-of-freedom are prescribed in the case of deformable nodes (OPTION1 = NODE or SET) whereas body rotations are prescribed in the case of a rigid body (OPTION1 = RIGID). In the case of a rigid body, the axis of prescribed rotation always passes through the body's center of mass. For |DOF| = 8, the axis of the prescribed rotation is parallel to vector VID. To prescribe a body rotation of a set of deformable nodes, with the axis of rotation parallel to global axes 𝑥, 𝑦, or 𝑧, use OPTION1 = SET with |DOF| = 9, 10, or 11, respectively. The load curve scale factor can be used for simple modifications or unit adjustments. The relative displacement can be measured in either of two ways: 1. Along a straight line between the mass centers of the rigid bodies, 2. Along a vector beginning at node 𝑛1 and terminating at node 𝑛2. With option 1, a positive displacement will move the rigid bodies further apart, and, likewise a negative motion will move the rigid bodies closer together. The mass centers of the rigid bodies must not be coincident when this option is used. With option 2 the relative displacement is measured along the vector, and the rigid bodies may be coincident. Note that the motion of the master rigid body is not directly affected by this option, i.e., no forces are generated on the master rigid body. The activation time, BIRTH, is the time during the solution that the constraint begins to act. Until this time, the prescribed motion card is ignored. The function value of the load curves will be evaluated at the offset time given by the difference of the solution time and BIRTH, i.e., (solution time-BIRTH). Relative displacements that occur prior to reaching BIRTH are ignored. Only relative displacements that occur after BIRTH are prescribed. When the constrained node is on a rigid body, the translational motion is imposed without altering the angular velocity of the rigid body by calculating the appropriate translational velocity for the center of mass of the rigid body using the equation: 𝐯cm = 𝐯node − 𝛚 × (𝐱cm − 𝐱node) where 𝐯𝑐𝑚 is the velocity of the center of mass, 𝐯node is the specified nodal velocity, 𝛚 is the angular velocity of the rigid body, 𝐱cm is the current coordinate of the mass center, and 𝐱node is the current coordinate of the nodal point. Extreme care must be used when prescribing motion of a rigid body node. Typically, for nodes on a given rigid body, the motion of no more than one node should be prescribed or unexpected results may be obtained. When the RIGID option is used to prescribe rotation of a rigid body, the axis of rotation will always be shifted such that it passes through the center-of-mass of the rigid body. By using *PART_INERTIA or *CONSTRAINED_NODAL_RIGID_BODY_INERTIA, one can override the internally-calculated location of the center-of-mass. When the RIGID_LOCAL option is invoked, the orientation of the local coordinate system rotates with time in accordance with rotation of the rigid body. Angular displacements are applied in an incremental fashion hence it is not possible to correctly prescribe a successive set of rotations about multiple axes. In light of this the command *BOUNDARY_PRESCRIBED_ORIENTATION_RIGID should be used for the purpose of prescribing the general orientation of a rigid body. Example: $$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ $ $$$$ *BOUNDARY_PRESCRIBED_MOTION_SET $ $$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ $ $ A set of nodes is given a prescribed translational velocity in the $ x-direction according to a specified vel-time curve (which is scaled). $ *BOUNDARY_PRESCRIBED_MOTION_SET $ $...>....1....>....2....>....3....>....4....>....5....>....6....>....7....>....8 $ nsid dof vad lcid sf vid death 4 1 0 8 2.0 $ $ nsid = 4 nodal set ID number, requires a *SET_NODE_option $ dof = 1 motion is in x-translation $ vad = 0 motion prescribed is velocity $ lcid = 8 velocity follows load curve 8, requires a *DEFINE_CURVE $ sf = 2.0 velocity specified by load curve is scaled by 2.0 $ vid not used in this example $ death use default (essentially no death time for the motion) $ $$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ $ $ $$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ $ $$$$ *BOUNDARY_PRESCRIBED_MOTION_RIGID $ $$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ $ $ A rigid body is given a prescribed rotational displacement about the $ z-axis according to a specified displacement-time curve. $ *BOUNDARY_PRESCRIBED_MOTION_RIGID $ $...>....1....>....2....>....3....>....4....>....5....>....6....>....7....>....8 $ pid dof vad lcid sf vid death 84 7 2 9 14.0 $ $ pid = 84 apply motion to part number 84 $ dof = 7 rotation is prescribed about the z-axis $ vad = 2 the prescribed motion is displacement (angular) $ lcid = 9 rotation follows load curve 9, requires a *DEFINE_CURVE $ (rotation should be in radians) $ sf use default (sf = 1.0) $ vid not used in this example $ death = 14 prescribed motion is removed at 14 ms (assuming time is in ms) $ $$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ $ SET_LINE option: Referring to Figure 5-4 and a partial keyword example below, a flat plate is being pulled along one edge while the opposite edge is fully constrained. All four existing nodes and new nodes created from h-adaptive mesh refinement along the straight line connecting nodes 98 and 105 will be included in a node set ID 122, which is subjected to a velocity boundary condition defined by load curve ID 2. From the deformed shape, it is evident all nodes are pulled equally according to the boundary condition. $$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ *BOUNDARY_PRESCRIBED_MOTION_SET_LINE $# nsid dof vad lcid sf vid death birth 122 3 0 2 $ NBEG NEND 98 105 $$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ *DEFINE_CURVE 0.0 &velo &endtime &velo 1000.0 &velo Revision Information: SET_LINE option is available starting in Revision 109996 for both SMP and MPP. All nodes fixed along this edge Undeformed mesh X Y Node 98 Node 105 All existing nodes along the straight line connecting nodes 98 and 105 are automatically included in the displacement boundary. A displacement boundary condition Node 105 Deformed mesh Node 98 New nodes created from adaptive refinement along the straight line connecting nodes 98 and 105 are also included in the displacement boundary. Figure 5-4. The SET_LINE option usage. *BOUNDARY_PRESCRIBED_ORIENTATION_RIGID_OPTION1_{OPTION2} Available options OPTION1 include: DIRCOS ANGLES EULERP VECTOR OPTION2 allows an optional ID: ID The defined ID can be referred to by *SENSOR_CONTROL. Purpose: Prescribe the orientation of rigid body as a function of time. Card Formats: ID Card. Optional card for ID keyword option. ID Variable 1 ID Type I 2 3 4 5 6 7 8 HEADING A70 Card 1 is common to all orientation methods. Cards 2 to 3 are unique for each orientation method. Card 1 1 2 3 4 5 6 7 8 Variable PIDB PIDA INTRP BIRTH DEATH TOFFSET Type I Default none I 0 I 1 F 0. F 1020 I VARIABLE ID DESCRIPTION Optional ID for PRESCRIBED ORIENTATION that can be referred to by *SENSOR_CONTROL. When not defined, the sequential definition order will be used as ID when referred to by *SENSOR_CONTROL. HEADING An optional descriptor for the given ID. PIDA Part ID for rigid body A. If zero then orientation of PIDB is performed with respect to the global reference frame. INTRP Interpolation method used on time history curves: EQ.1: linear interpolation (default) EQ.2: cubic spline development) interpolation (experimental – under BIRTH DEATH Prior to this time the body moves freely under the action of other agents. The body is freed at this time and subsequently allowed to move under the action of other agents. TOFFSET Time offset flag: EQ.1: The time value of all load curves will be offset by the birth time. EQ.0: No time offset is applied. Cosine Card 1. Additional card for DIRCOS option. Card 2 1 2 3 4 5 6 7 8 Variable LCIDC11 LCIDC12 LCIDC13 LCIDC21 LCIDC22 LCIDC23 LCIDC31 LCIDC32 Type I I I I I I I I Default none none none none none none none none Cosine Card 2. Additional card for DIRCOS option. Card 3 1 2 3 4 5 6 7 8 Variable LCIDC33 Type I Default none VARIABLE LCIDCij DESCRIPTION Load curve ID specifying direction cosine 𝐶𝑖𝑗 as a function of time. 𝐶𝑖𝑗 is defined as: 𝐶𝑖𝑗 = 𝐚𝑖 ⋅ 𝐛𝑗 where the {𝒂𝑖} are mutually perpendicular unit vectors fixed in PIDA and the {𝒃𝑗} are mutually perpendicular unit vectors fixed in PIDB. If PIDA = 0 then the {𝒂𝑖} are unit vectors aligned with the global 𝑥, 𝑦, and 𝑧. See Remark 1. Angles Card. Additional card for ANGLES option. Card 2 1 2 3 4 5 6 7 8 Variable LCIDQ1 LCIDQ2 LCIDQ3 ISEQ ISHFT BODY Type I I I I Default none none none none I 1 I 0 VARIABLE LCIDQi ISEQ DESCRIPTION Load curve ID specifying the orientation angle 𝑞𝑖 in radians as a function of time. See Remark 1. Specifies the sequence in which the rotations are performed. In this first set of sequences three unique axes are involved. This sequence is associated with what are commonly called Cardan or Tait-Bryan angles. All angles are in units of radians. Whether these rotations are intrinsic or extrinsic is determined by the BODY field. EQ.123: The first rotation is performed about the 𝑥 axis through an angle of 𝑞1, the second about the 𝑦 axis through an angle of 𝑞2, and the third about the 𝑧 axis through an angle of 𝑞3. EQ.231: The first rotation is performed about the 𝑦 axis through an angle of 𝑞1, the second about the 𝑧 axis through an angle of 𝑞2, and the third about the 𝑥 axis through an angle of 𝑞3. EQ.312: The first rotation is performed about the 𝑧 axis through an angle of 𝑞1, the second about the 𝑥 axis through an angle of 𝑞2, and the third about the 𝑦 axis through an angle of 𝑞3. EQ.132: The first rotation is performed about the 𝑥 axis through an angle of 𝑞1, the second about the 𝑧 axis through an angle of 𝑞2, and the third about the 𝑦 axis through an angle of 𝑞3. EQ.213: The first rotation is performed about the 𝑦 axis through an angle of 𝑞1, the second about the 𝑥 axis through an angle of 𝑞2, and the third about the 𝑧 axis through an angle of 𝑞3. EQ.321: The first rotation is performed about the 𝑧 axis through an angle of 𝑞1, the second about the 𝑦 axis through an angle of 𝑞2, and the third about the 𝑧 axis through an angle of 𝑞3. The second set of sequences involve only two unique axes where the first and third are repeated. This sequence is associated with what are commonly called Euler angles. EQ.121: the first rotation is performed about the 𝑥 axis through an angle of 𝑞1, the second about the 𝑦 axis through an angle of 𝑞2, and the third about the 𝑥 axis through an angle of 𝑞3. EQ.131: The first rotation is performed about the 𝑥 axis through an angle of 𝑞1, the second about the 𝑧 axis through an angle of 𝑞2, and the third about the 𝑥 axis through an angle of 𝑞3. EQ.212: The first rotation is performed about the 𝑦 axis through an angle of 𝑞1, the second about the 𝑥 axis through an angle of 𝑞2, and the third about the 𝑦 axis through an angle of 𝑞3. EQ.232: The first rotation is performed about the 𝑦 axis through an angle of 𝑞1, the second about the 𝑧 axis through an angle of 𝑞2, and the third about the 𝑦 axis through an angle of 𝑞3. EQ.313: The first rotation is performed about the 𝑧 axis through an angle of 𝑞1, the second about the 𝑥 axis through an angle of 𝑞2, and the third about the 𝑧 axis through an angle of 𝑞3. EQ.323: The first rotation is performed about the 𝑧 axis through an angle of 𝑞1, the second about the 𝑦 axis through an angle of 𝑞2, and the third about the 𝑧 axis through an angle of 𝑞3. ISHFT Angle shift. EQ.1: Angle curves are unaltered. EQ.2: Shifts angle data in the LCIDQi curves as necessary to eliminate discontinuities. If angles are confined to the range [−𝜋, 𝜋] and the data contains excursions exceeding 𝜋 then set ISHFT = 2. BODY Reference axes. EQ.0: Rotations are performed about axes fixed in PIDA (extrinsic rotation, default). EQ.1: Rotations are performed about axes fixed in PIDB (intrinsic rotation). Euler Parameter Card. Additional card for EULERP option. Card 2 1 2 3 4 5 6 7 8 Variable LCIDE1 LCIDE2 LCIDE3 LCIDE4 Type I I I I Default none none none none VARIABLE LCIDEi DESCRIPTION Load curve ID specifying Euler parameter 𝑒𝑖 as a function of time. The Euler parameters are defined as follows. See Remark 1. 𝜀𝑖 = 𝜺 ⋅ 𝒂𝑖 = 𝜺 ⋅ 𝒃𝑖, (𝑖 = 1, 2, 3) 𝜀4 = cos ( ) where 𝜺 is the Euler vector, {𝒂𝑖} and {𝒃𝑖} are dextral sets of unit vectors fixed in PIDA and PIDB, respectively, and 𝜃 (in radians) is associated with the rotation of PIDB in PIDA about Euler vector. If PIDA = 0 then the {𝒂𝑖} are unit vectors aligned, respectively, with the global 𝑥, 𝑦, and 𝑧 axes. 2)𝒏 and 𝜀4 = cos(𝜃 The Euler parameters are defined as 𝜺 = sin(𝜃 2), respectively. Here 𝒏 is a unit vector defining the axis of rotation, and 𝜃 is the angle with which the rotation 2 = occurs, and consequently the four parameters are subjected to the condition 𝛆𝑇𝛆 + 𝜀4 1. It is therefore recommended that the control points of the curves already fulfil this or else LS-DYNA will internally normalize these values. From the Euler parameters at time 𝑡, a unique rotation matrix 𝑸𝑡 is computed that is used to determine the total orientation 𝑸. The rotation is performed with respect to the reference state 𝑸0 given by the Euler parameters at time 0. In general, 𝑸0 ≠ 𝑰 and the rotation of the rigid body is 𝑇. If the parameters are initially 𝜺 = 𝟎 and 𝜀4 = 1, then the reference given by 𝑸 = 𝑸𝑡𝑸0 state is 𝑸0 = 𝑰 and 𝑸 = 𝑸𝑡 defines the orientation of the rigid body. For a nonzero PIDA, the rotation matrix 𝑸 as defined above is expressed in a system that is fixed in rigid body A. If this system is denoted 𝑹𝑡 at time 𝑡, and assuming 𝑹0 = 𝑰, the orientation with respect to a global system is 𝑹𝑸. Vector Card. Additional card for VECTOR option. Card 2 1 2 3 4 5 6 7 8 Variable LCIDV1 LCIDV2 LCIDV3 LCIDS VALSPIN Type I I I Default none none none I 0 F 0. VARIABLE LCIDVi DESCRIPTION Load curve ID specifying the vector measure number 𝑣𝑖 as a function of time. The vector measure numbers are defined as follows. See Remark 1. 𝑣𝑖 = 𝒗 ⋅ 𝒏𝑖, 𝑖 = 1, 2, 3. where 𝒗 is a vector and {𝒏𝑖} are unit vectors aligned, respectively, with the global axes 𝑥, 𝑦, and 𝑧 axes. Note that the vector 𝒗 is attached to the body in question, so changing the direction of this vector will induce a rotation of the body defined by 𝝋̇ = 𝒗 × 𝒗̇. LCIDS Load curve ID which specifies the overlayed spin speed 𝜃̇ of PIDB about the axis parallel to the vector 𝒗. EQ.0: a constant spin speed as defined by VALSPIN is used, GT.0: Load curve for spin speed (radians per unit time). VALSPIN Value for the constant spin speed of PIDB (radians per unit time 𝜃̇). This option is bypassed if the load curve number defined above is non-zero. 𝜃̇ 𝑛 𝒗𝑛 Time 𝑡𝑛 𝜃̇ 𝑛+1 𝒗𝑛+1 Time 𝑡𝑛+1 Total spin 𝝎 given by 𝝎 = 𝝋̇ + 𝜽̇ = 𝒗 × 𝒗̇ + 𝜃̇𝒗 Remarks: 1. All load curves must contain the same number of points and the data must be uniformly spaced. 2. LC0 in *MAT_RIGID must be used to identify a coordinate system for each rigid body. The coordinate system must be defined with *DEFINE_COORDI- NATE_NODES and FLAG = 1. Nodes used in defining the coordinate system must reside on the same body. 3. This feature is incompatible with *DEFINE_CURVE_FUNCTION. *BOUNDARY_PRESSURE_OUTFLOW_OPTION Available options include: SEGMENT SET Purpose: Define pressure outflow boundary conditions. These boundary conditions are attached to solid elements using the Eulerian ambient formulation (refer to ELFORM in *SECTION_SOLID_ALE) and defined to be pressure outflow ambient elements (refer to AET in *SECTION_SOLID_ALE). Card 1 for SET option. Card 1 1 2 3 4 5 6 7 8 Variable SSID Type I Default none Card 1 for SEGMENT option. Card 1 Variable 1 N1 Type I 2 N2 I 3 N3 I 4 N4 I Default none none none none 5 6 7 8 VARIABLE DESCRIPTION SSID Segment set ID N1, N2, … Node ID’s defining segment *BOUNDARY_PWP_OPTION Available options include: NODE SET TABLE TABLE_SET Purpose: Define pressure boundary conditions for pore water, e.g. at soil surface. The TABLE option applies to a whole Part, while the other options apply to specified nodes. Card 1 1 Variable typeID Type I 2 LC F 3 4 5 6 7 8 CMULT LCDR TBIRTH TDEATH F I F F Default none none 0.0 none 0.0 1020 Card 2 1 2 3 4 5 6 7 8 Variable IPHRE ITOTEX IDRFLAG TABLE Type Default I 0 I 0 I 0 I 0 VARIABLE DESCRIPTION typeID LC Node ID (option = NODE) or Node set ID (option = SET) or Part ID (option = TABLE) or Part Set ID (option = TABLE_SET) Load curve or function giving pore water pressure head (length units) vs time. EQ.0: constant pressure head assumed equal to CMULT (leave blank for TABLE option) VARIABLE DESCRIPTION CMULT Factor on curve or constant pressure head if LC = 0 LCDR Load curve or function giving pore water pressure head during dynamic relaxation. EQ.0: during dynamic relaxation, use first pressure head value on LC (leave blank for TABLE option) TBIRTH Time at which boundary condition becomes active TDEATH Time at which boundary condition becomes inactive IPHRE EQ.0: default behavior EQ.1: for phreatic behavior (water can be removed by the boundary condition but not added, e.g. at a sloping free surface). Not applicable to TABLE option. See remarks. ITOTEX Flag for type of pressure boundary condition: EQ.0: Total head EQ.1: Excess head EQ.2: Hydraulic head EQ.4: 𝑧-coord where head = 0 (piezometric level) IDRFLAG Active flag: EQ.0: Active only in transient analysis EQ.1: Active only in dynamic relaxation EQ.2: Active in all analysis phases (leave blank for TABLE option) TABLE Table ID for TABLE option only. See notes below. Remarks: 1. Pressure is given as pressure head, i.e. pressure/ρg. 2. NODE and SET options do not affect the pore pressure in Drained parts (the pore pressure for these is set on a part basis and overrides any nodal boundary conditions). The TABLE option should be used only with Drained parts. 3. 4. *BOUNDARY_PWP_NODE or SET overrides pressure head from *BOUND- ARY_PWP_TABLE at nodes where both are present. 4. If LC is a *DEFINE_FUNCTION, the input arguments are (time, x, y, z, x0, y0, z0) where x, y and z are the current coordinates and x0, y0, z0 are the initial coordinates of the node. TABLE and TABLE_SET options: The table consists of a list of times in ascending order, followed immediately by curves of 𝑧-coordinate versus pore pressure head. Each curve represents the pore water pressure head distribution with 𝑧-coordinate at the corresponding time. There must be the same number of curves as time values, arranged immediately after the *DEFINE_- TABLE and in the correct order to correspond to the time values. Each curve should be arranged in ascending order of 𝑧-coordinate – they look upside-down on the page. The 𝑧-coordinate is the 𝑥-axis of the curve, the pore water pressure head (in length units) is the y-axis. Each curve should have the same 𝑧-coordinates (𝑥-values) and use the same value of LCINT. Ensure that the range of 𝑧-coordinates in the curve exceeds by at least 5% the range of 𝑧-coordinates of the nodes belonging to the parts to which the boundary condition is applied. IPHRE: “Phreatic” means that water can be removed by the boundary condition but not added. The boundary condition enforces that the pressure head be less than or equal to the stated value. This condition occurs when the free surface of the soil is sloping so that any water emerging from the soil runs away down the slope. ITOTEX = 0: The value from curve or table is total head. This may be used with any pore pressure analysis type. ITOTEX = 1: The value from curve or table is excess head. Total head will be determined by adding the hydrostatic head. This option cannot be used with drained analysis, which sets excess head to zero. ITOTEX = 2: The value from curve or table is hydraulic head, to which excess head may be added due to volume change in the soil if the analysis type is not drained. *BOUNDARY The curve value is the z-coordinate of the water surface; pore pressure head at any node in this boundary condition is given by, 𝑧surface − 𝑧node This option allows a single boundary condition to be used for nodes at any depth, provided that the pressure distribution is hydrostatic below the given surface. This option is not available for the TABLE option. *BOUNDARY_RADIATION_OPTION1_{OPTION2}_{OPTION3} Available values for OPTION1 include: SET SEGMENT Available values for OPTION2 include: VF_READ VF_CALCULATE <BLANK> Available values for OPTION3 include: RESTART <BLANK> OPTION1 specifies radiation boundary surface definition by a surface set (SET) or by a segment list (SEGMENT). OPTION2 indicates the radiation boundary surface is part of an enclosure. When set to VF OPTION2 specifies the use of view factors. The suffix, READ, indicates that the view factors should be read from the file “viewfl”. The suffix, CALCULATE, indicates that the view factors should be calculated. The Stefan Boltzmann constant must be defined for radiation in an enclosure on the *CONTROL_THERMAL_SOLVER keyword. The parameter DTVF entered on the CONTROL_THERMAL_SOLVER keyword defines the time interval between VF updates for moving geometries. OPTION3 is the keyword suffix RESTART. This is only applicable in combination with the keyword VF_CALCULATE. In very long runs, it may be necessary to halt execution. This is accomplished by entering Ctrl-C followed by sw1. To restart the view factor calculation, add the suffix RESTART to all VF_CALCULATE keywords in the input file. The status of an in-progress view factor calculation can be determined by using the sense switch. This is accomplished by first typing Control-C followed by: sw1. sw2. Stop run and save viewfl file for restart Viewfactor run statistics A list of acceptable keywords are: *BOUNDARY_RADIATION_SEGMENT *BOUNDARY_RADIATION_SEGMENT_VF_READ *BOUNDARY_RADIATION_SEGMENT_VF_CALCULATE *BOUNDARY_RADIATION_SET *BOUNDARY_RADIATION_SET_VF_READ *BOUNDARY_RADIATION_SET_VF_CALCULATE Remarks: In models that include radiation boundary conditions, a thermodynamic temperature scale is required, i.e., zero degrees must correspond to absolute zero. The Kelvin and Rankine temperature scales meet this requirement whereas Celsius and Fahrenheit temperature scales do not. *BOUNDARY_RADIATION_SEGMENT Include the following 2 cards for each segment. Apply a radiation boundary condition on a SEGMENT to transfer heat between the segment and the environment. Setting TYPE = 1 on Card 1 below indicates that the segment transfers heat to the environment. Card 1 Variable 1 N1 Type I 2 N2 I 3 N3 I 4 N4 I Default none none none none Card 2 1 2 3 4 5 6 7 8 TYPE I 1 5 6 7 8 Variable FLCID FMULT TLCID TMULT LOC Type I F I F Default none 0. none 0. I 0 VARIABLE DESCRIPTION N1, N2, N3, N4 TYPE FLCID Node ID’s defining segment Radiation type: EQ.1: Radiation to environment Radiation heat transfer coefficient, 𝑓 = 𝜎𝜀𝐹, specification where σ = Stefan Boltzmann constant, ε = surface emissivity, F = surface view factor. This parameter can reference a load curve ID or a function ID . When the reference is to a curve, FLCID has the following interpretation: GT.0: 𝑓 is defined as a function of time, 𝑡, having points consisting of (𝑡, 𝑓 (𝑡)) data pairs. EQ.0: 𝑓 is a constant defined by the value FMULT. VARIABLE DESCRIPTION LT.0: 𝑓 is defined as a function of temperature, 𝑇, by a curve consisting of (𝑇, 𝑓 (𝑇) ) data pairs. Enter |FLCID| on the DEFINE_CURVE keyword. FMULT Radiation heat transfer coefficient, f, curve multiplier for use in the equation q̇′′ = 𝜎𝜀𝐹(𝑇surface − 𝑇∞ 4 ) = 𝑓 (𝑇surface − 𝑇∞ 4 ) TLCID If f is a function of temperature, f is evaluated at the surface temperature, Tsurface. [σ = Stefan Boltzmann constant, ε = surface emissivity, F = surface view factor] Environment temperature, 𝑇∞, specification. This parameter can reference a load curve ID or a function ID . When the reference is to a curve, TLCID has the following interpretation: GT.0: 𝑇∞ is defined as a function of time, 𝑡, by a curve consisting of (𝑡, 𝑇∞(𝑡) ) data pairs. EQ.0: 𝑇∞ a constant defined by the value TMULT. TMULT Environment temperature, 𝑇∞, curve multiplier. LOC For a thick thermal shell, the radiation will be applied to the surface identified by LOC. See the parameter THSHEL on the *CONTROL_SHELL keyword. EQ.-1: lower surface of thermal shell element EQ.0: middle surface of thermal shell element EQ.1: upper surface of thermal shell element Remarks: A radiation boundary condition is calculated using q̇′′ = 𝜎𝜀𝐹(𝑇surface − 𝑇∞ 4 ) = 𝑓 (𝑇surface − 𝑇∞ 4 ) Where, 𝑓 , is the radiation heat transfer coefficient. If 𝑓 is a function of temperature, 𝑓 , is evaluated at the surface temperature, Tsurface. 1. If HLCID references a DEFINE_FUNCTION, the following function arguments are allowed 𝑓 (𝑥, 𝑦, 𝑧, 𝑣𝑥, 𝑣𝑦, 𝑣𝑧, 𝑇, 𝑇∞, 𝑡) where: 𝑥, 𝑦, 𝑧 = segment centroid coordinates 𝑣𝑥, 𝑣𝑦, 𝑣𝑧 = segment centroid velocity component T = segment centroid temperature 𝑇∞ = environment temperature, T∞ 𝑡 = solution time 2. If TLCID references a DEFINE_FUNCTION, the following function arguments are allowed 𝑓 ( 𝑥 , 𝑦 , 𝑧 , 𝑣𝑥, 𝑣𝑦, 𝑣𝑧, 𝑡) where: 𝑥, 𝑦, 𝑧 = segment centroid coordinates 𝑣𝑥, 𝑣𝑦, 𝑣𝑧 = segment centroid velocity components 𝑡 = solution time *BOUNDARY_RADIATION_SEGMENT_VF_OPTION Available options include: READ CALCULATE Include the following 2 cards for each segment. Apply a radiation boundary condition on a SEGMENT to transfer heat between the segment and an enclosure surrounding the segment using view factors. The enclosure is defined by additional segments using this keyword. Setting TYPE = 2 on Card 1 below specifies that the segment belongs to an enclosure. The file “viewfl” must be present for the READ option, whereas it will be created with the CALCULATE option. If the file “viewfl” exists when using the CALCULATE option, LS-DYNA will terminate with an error message to prevent overwriting the file. The file “viewfl” contains the surface-to-surface area × view factor products (i.e., 𝐴𝑖𝐹𝑖𝑗). These products are stored by row and formatted as 5E16.0. Card 1 Variable 1 N1 Type I 2 N2 I 3 N3 I 4 N4 I Default none none none none Card 2 1 2 3 4 5 6 7 8 TYPE BLOCK NINT I 2 5 I 0 6 I 0 7 8 Variable SELCID SEMULT Type I F Default none 0. VARIABLE DESCRIPTION N1, N2, N3, N4 Node ID’s defining segment VARIABLE DESCRIPTION TYPE Radiation type: EQ.2: Radiation within an enclosure BLOCK Flag indicating if this surface blocks the view between any other 2 surfaces. EQ.0: no blocking (default) EQ.1: blocking NINT Number of integration points for viewfactor calculation EQ.0: LS-DYNA determines the number of integration points based on the segment size and separation distance 1 ≤ NINT ≤ 10: User specified number SELCID Load curve ID for surface emissivity, see *DEFINE_CURVE GT.0: function versus time EQ.0: use constant multiplier value, SEMULT LT.0: function versus temperature. The value of –SELCID must be an integer, and it is interpreted as a load curve ID. See the DEFINE_CURVE keyword. SEMULT Curve multiplier for surface emissivity, see *DEFINE_CURVE *BOUNDARY Include the following 2 cards for each set. Apply a radiation boundary condition on a SEGMENT_SET to transfer heat between the segment set and the environment Setting TYPE = 1 on Card 1 below indicates that the segment transfers energy to the environment. Card 1 1 2 3 4 5 6 7 8 Variable SSID TYPE Type I Default none Card 2 1 I 1 2 3 4 5 6 7 8 Variable FLCID FMULT TLCID TMULT LOC Type I F I F Default none 0. none 0. I 0 VARIABLE SSID DESCRIPTION SSID specifies the ID for a set of segments that comprise a portion of, or possibly, the entire enclosure. See *SET_SEGMENT. TYPE Radiation type: EQ.1: Radiation to environment FLCID Radiation heat transfer coefficient, 𝑓 = 𝜎𝜀𝐹, specification where σ = Stefan Boltzmann constant, ε = surface emissivity, F = surface view factor. This parameter can reference a load curve ID or a function ID . When the reference is to a curve, FLCID has the following interpretation: GT.0: 𝑓 is defined as a function time, 𝑡, by a curve consisting of (𝑡, 𝑓 (𝑡)) data pairs. VARIABLE DESCRIPTION EQ.0: 𝑓 is a constant defined by the value FMULT. LT.0: 𝑓 is defined as a function of temperature, 𝑇, by a curve consisting of (𝑇, 𝑓 (𝑇)) data pairs. Enter |-FLCID| on the DEFINE_CURVE keyword FMULT Curve multiplier for f for use in the equation q̇′′ = 𝜎𝜀𝐹(𝑇surface − 𝑇∞ 4 ) = 𝑓 (𝑇surface − 𝑇∞ 4 ) TLCID If f is a function of temperature, f is evaluated at the surface temperature, Tsurface. [σ = Stefan Boltzmann constant, ε = surface emissivity, F = surface view factor] Environment temperature, 𝑇∞ , specification. This parameter can reference a load curve ID or a function ID . When the reference is to a curve, TLCID has the following interpretation: GT.0: 𝑇∞ is defined as a function of time, 𝑡, by a curve consisting of (𝑡, 𝑇∞(𝑡)) data pairs. EQ.0: 𝑇∞ a constant defined by the value TMULT TMULT Curve multiplier for 𝑇∞ LOC For a thick thermal shell, the radiation will be applied to the surface identified by LOC. See the parameter THSHEL on the *CONTROL_SHELL keyword. EQ.-1: lower surface of thermal shell element EQ.0.: middle surface of thermal shell element EQ.1: upper surface of thermal shell element Remarks: A radiation boundary condition is calculated using q̇′′ = 𝜎𝜀𝐹(𝑇surface − 𝑇∞ 4 ) = 𝑓 (𝑇surface − 𝑇∞ 4 ) Where, f , is the radiation heat transfer coefficient. . If f is a function of temperature, f, is evaluated at the surface temperature, Tsurface. 1. If HLCID references a DEFINE_FUNCTION, the following function arguments are allowed 𝑓 (𝑥, 𝑦, 𝑧, 𝑣𝑥, 𝑣𝑦, 𝑣𝑧, 𝑇, 𝑇∞, 𝑡) where: 𝑥, 𝑦, 𝑧 = segment centroid coordinates 𝑣𝑥, 𝑣𝑦, 𝑣𝑧 = segment centroid velocity component 𝑇 = segment centroid temperature 𝑇∞ = environment temperature, T∞ 𝑡 = solution time 2. If TLCID references a DEFINE_FUNCTION, the following function arguments are allowed 𝑓 (𝑥, 𝑦, 𝑧, 𝑣𝑥, 𝑣𝑦, 𝑣𝑧, 𝑡) where: 𝑥, 𝑦, 𝑧 = segment centroid coordinates 𝑣𝑥, 𝑣𝑦, 𝑣𝑧 = segment centroid velocity components 𝑡 = solution time *BOUNDARY_RADIATION_SET_VF_OPTION Available options include: READ CALCULATE Include the following 2 cards for each set. Apply a radiation boundary condition on a SEGMENT_SET to transfer heat between the segment set and an enclosure surrounding the segments using view factors. Segments contained in the SEGMENT_SET may form the enclosure. Setting TYPE = 2 on Card 1 below specifies that the segment set belongs to an enclosure. The file “viewfl” must be present for the READ option. The file “viewfl” will be created for the CALCULATE option. If the file “viewfl” exists when using the CACULATE option, LS-DYNA will terminate with an error message to prevent overwriting the file. The file “viewfl” contains the surface-to-surface area × view factor products (i.e. 𝐴𝑖𝐹𝑖𝑗). These products are stored by row and formatted as 5E16.0. Card 1 1 2 3 4 5 6 7 8 Variable SSID TYPE RAD_GRP FILE_NO BLOCK NINT Type I Default none Card 2 1 I 2 2 I 0 3 I 0 4 I 0 5 I 0 6 7 8 Variable SELCID SEMULT Type I F Default none 0. VARIABLE SSID DESCRIPTION SSID specifies the ID for a set of segments that comprise a portion of, or possibly, the entire enclosure. See *SET_SEGMENT. VARIABLE DESCRIPTION TYPE Radiation type: EQ.2: Radiation within an enclosure RAD_GRP FILE_NO Radiation enclosure group ID. The segment sets from all radiation enclosure definitions with the same group ID are augmented to form a single enclosure definition. If RAD_GRP is not specified or set to zero, then the segments are placed in group zero. All segments defined by the SEGMENT option are placed in set zero. File number for view factor file. FILE_NO is added to “viewfl_” to form the name of the file containing the view factors. For example if FILE_NO is specified as 22, then the view factors are read from viewfl_22. For radiation enclosure group zero FILE_- NO is ignored and view factors are read from viewfl. The same file may be used for different radiation enclosure group definitions. BLOCK Flag indicating if this surface blocks the view between any other 2 surfaces. EQ.0: no blocking (default) EQ.1: blocking NINT Number of integration points for viewfactor calculation EQ.0: LS-DYNA determines the number of integration points based on the segment size and separation distance GE.11: Not allowed SELCID Load curve ID for surface emissivity, see *DEFINE_CURVE GT.0: function versus time EQ.0: use constant multiplier value, SEMULT LT.0: function versus temperature. Enter –SELCID as |- SELCID| on the DEFINE_CURVE keyword. SEMULT Curve multiplier for surface emissivity, see *DEFINE_CURVE *BOUNDARY_RADIATION_SET_VF Multiple enclosures can be modeled when using view factors. Consider the following example input. The order of segments in the view factor file follows the order the sets are assigned to the boundary radiation definition. $$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ $ $$$$ *BOUNDARY_RADIATION_SET $ $$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ $ $ Make boundary enclosure radiation groups 8 and 9. $ *BOUNDARY_RADIATION_SET_VF_READ * SSID TYPE RAD_GRP FILE_NO 15 2 9 10 1.0 1.0 *BOUNDARY_RADIATION_SET_VF_READ * SSID TYPE RAD_GRP FILE_NO 12 2 9 10 1.0 1.0 *BOUNDARY_RADIATION_SET_VF_READ * SSID TYPE RAD_GRP FILE_NO 13 2 8 21 1.0 1.0 $ $ $$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ Enclosure radiation group 9 is composed of all the segments in segment set 15 followed by those in segment set 12. The view factors are stored in the file viewfl_10. Enclosure radiation group 8 is composed of the segments in segment set 13. The view factors are stored in the file viewfl_21. *BOUNDARY Purpose: Define a sliding symmetry plane. This option applies to continuum domains modeled with solid elements. Card 1 1 Variable NSID Type I Default none 2 VX F 0 3 VY F 0 4 VZ F 0 5 6 7 8 COPT I 0 VARIABLE DESCRIPTION NSID Nodal set ID, see *SET_NODE VX VY VZ x-component of vector defining normal or vector y-component of vector defining normal or vector z-component of vector defining normal or vector COPT Option: EQ.0: node moves on normal plane, EQ.1: node moves only in vector direction. Remarks: Any node may be constrained to move on an arbitrarily oriented plane or line depending on the choice of COPT. Each boundary condition card defines a vector originating at (0, 0, 0) and terminating at the coordinates defined above. Since an arbitrary magnitude is assumed for this vector, the specified coordinates are non- unique and define only a direction. Use of *BOUNDARY_SPC is preferred over *BOUNDARY_SLIDING_PLANE as the boundary conditions imposed via the latter have been seen to break down somewhat in lengthy simulations owing to numerical roundoff. *BOUNDARY_SPC_OPTION1_{OPTION2}_{OPTION3} OPTION1 is required since it specifies whether the SPC applies to a single node or to a set. The two choices are: NODE SET OPTION2 allows optional birth and death times to be assigned the single node or node set: BIRTH_DEATH This option requires one additional line of input. The BIRTH_DEATH option is inactive during the dynamic relaxation phase, which allows the SPC to be removed during the subsequent normal analysis phase. The BIRTH_DEATH option can be used only once for any given node and if used, no other *BOUNDARY_SPC commands can be used for that node. OPTION3 allows an optional ID to be given that applies either to the single node or to the entire set: ID If a heading is defined with the ID, then the ID with the heading will be written at the beginning of the ASCII file, spcforc. Purpose: Define nodal single point constraints. Do not use this option in r-adaptive problems since the nodal point ID's change during the adaptive step. If possible use CONSTRAINED_GLOBAL instead. ID Card. Additional card for the ID keyword option. Optional Variable 1 ID Type I 2 3 4 5 6 7 8 HEADING A70 Card 1 1 2 3 4 5 6 7 8 Variable NID/NSID CID DOFX DOFY DOFZ DOFRX DOFRY DOFRZ Type I Default none I 0 I 0 I 0 I 0 I 0 I 0 I 0 Birth/Death Card. Additional card for the BIRTH_DEATH keyword option. Card 2 1 2 3 4 5 6 7 8 Variable BIRTH DEATH Type F F Default 0.0 1020 VARIABLE DESCRIPTION ID Optional SPC set ID to which this node or node set belongs. This ID does not need to be unique HEADING An optional SPC descriptor that will be written into the d3hsp file and the spcforc file. NID/NSID Node ID or nodal set ID, see *SET_NODE. CID DOFX DOFY DOFZ Coordinate system ID, see *DEFINE_COORDINATE_SYSTEM. Insert 1 for translational constraint in local 𝑥-direction. Insert 1 for translational constraint in local 𝑦-direction. Insert 1 for translational constraint in local 𝑧-direction. DOFRX Insert 1 for rotational constraint about local 𝑥-axis. DOFRY Insert 1 for rotational constraint about local 𝑦-axis. DOFRZ Insert 1 for rotational constraint about local 𝑧-axis. VARIABLE DESCRIPTION Activation time for SPC constraint. The birth time is ignored during dynamic relaxation. Deactivation time for the SPC constraint. The death time is ignored during dynamic relaxation. BIRTH DEATH Remarks: Constraints are applied if for each DOFij field set to 1. A value of zero means no constraint. No attempt should be made to apply SPCs to nodes belonging to rigid bodies . $$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ $ $$$$ *BOUNDARY_SPC_NODE $ $$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ $ $ Make boundary constraints for nodes 6 and 542. $ *BOUNDARY_SPC_NODE $ $...>....1....>....2....>....3....>....4....>....5....>....6....>....7....>....8 $ nid cid dofx dofy dofz dofrx dofry dofrz 6 0 1 1 1 1 1 1 542 0 0 1 0 1 0 1 $ $ Node 6 is fixed in all six degrees of freedom (no motion allowed). $ $ Node 542 has a symmetry condition constraint in the x-z plane, $ no motion allowed for y translation, and x & z rotation. $ $$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ *BOUNDARY_SPC_SYMMETRY_PLANE_{OPTION} This keyword is developed to create nodal symmetric constraints by defining a symmetric plane. Available options include: <BLANK> SET The option SET allows for symmetric boundary conditions to be applied on tailor- welded blanks (TWB). Card Sets. For each symmetry plane input one pair of cards 1 and 2. This input ends at the next keyword (“*”) card. Card 1 1 2 Variable IDSP PID/PSID Type I I 3 X F 4 Y F 5 Z F 6 VX F 7 VY F 8 VZ F Default none none 0.0 0.0 0.0 0.0 0.0 0.0 Card 2 1 2 3 4 5 6 7 8 Variable TOL Type F Default 0.0 VARIABLE DESCRIPTION IDSP Identification number of the constraint. Must be unique. PID/PSID A part ID of the deformable part (sheet metal blank, for example) on which the constraints will be imposed. When the option SET is invoked, a part set ID can be input. VX, VY, VZ X, Y, Z TOL TOL All nodes within +/- TOL of the plane defined by the point with coordinate (X, Y, Z) and the plane with normal vector (VX, VY, VZ) will be constrained symmetrically. Figure 5-5. Define symmetry constraints using the variables in the keyword. VARIABLE DESCRIPTION X, Y, Z Position coordinates on the symmetry plane. VX, VY, VZ Vector components of the symmetry plane normal. TOL A distance tolerance value within which the nodes on the deformable part will be constrained. Remarks: 1. Adaptive refined nodes generated along the symmetry plane during simulation are automatically included in the constraints. 2. Figure 5-5 shows an example of applying symmetry constraints using the variables in the keyword. 3. The following keyword creates symmetric constraints on nodes (from PID 11) within distance of 0.1mm from the defined symmetry plane (with normal vec- tors [1.0,1.0,1.0]) that goes through point coordinates (10.5, 40.0, 20.0): *BOUNDARY_SPC_SYMMETRY_PLANE $...>....1....>....2....>....3....>....4....>....5....>....6....>....7....>....8 $ IDSP PID X Y Z VX VY VZ 1 11 10.5 40.0 20.0 1.0 1.0 1.0 $...>....1....>....2....>....3....>....4....>....5....>....6....>....7....>....8 $ TOL 4. The following keywords create two symmetric constraints on nodes from part set ID 99 (which includes part IDs 13 and 14) within distance of 0.1mm from two defined symmetry planes (with normal vectors [1.0, 0.0, 0.0] and [0.0, 1.0, 0.0], respectively) that all go through point coordinates (-76.0, 35.6, 0.0). Note the two point coordinates that define the two symmetry planes must be exactly the same. *SET_PART_LIST 99 13,14 *BOUNDARY_SPC_SYMMETRY_PLANE_SET $ IDSP PID X Y Z VX VY VZ 1 99 -76.0 35.6 0.0 1.0 $ TOL 0.10 2 99 -76.0 35.6 0.0 0.0 1.0 $ TOL 0.10 Revision information: This feature is available starting in Revision 85404. The option SET is available starting in Revision 113355. *BOUNDARY_SPH_FLOW Purpose: Define a flow of particles. This option applies to continuum domains modeled with SPH elements. Card 1 Variable 1 ID 2 3 4 5 STYP DOF VAD LCID 6 SF F 7 8 DEATH BIRTH F F I none 1. 1.E+20 0.0 5 6 7 8 I 0 4 Type I I I Default none none none Card 2 1 2 3 Variable NODE VID Type I Default none I 0 VARIABLE NSID, PID DESCRIPTION Nodal set ID (NSID), SEE *SET_NODE, or part ID (PID), see *PART. STYP Set type: EQ.1: part set ID, see *SET_PART, EQ.2: part ID, see *PART, EQ.3: node set ID, see *NODE_SET, Node boundary vector VID deactivated particle activated particle SPH Flow Figure 5-6. Vector VID determines the orientation of the SPH flow VARIABLE DESCRIPTION DOF Applicable degrees-of-freedom: EQ.1: x-translational degree-of-freedom, EQ.2: y-translational degree-of-freedom, EQ.3: z-translational degree-of-freedom, EQ.4: translational motion in direction given by the VID. Movement on plane normal to the vector is permitted. VAD Velocity/Acceleration/Displacement elements before activation: flag applied to SPH EQ.0: velocity, EQ.1: acceleration, EQ.2: displacement. LCID Load curve ID to describe motion value versus time, see *DE- FINE_CURVE. SF Load curve scale factor. (default = 1.0) DEATH Time imposed motion/constraint is removed: EQ.0.0: default set to 1020. BIRTH Time imposed motion/constraint is activated. VARIABLE NODE DESCRIPTION Node fixed in space which determines the boundary between activated particles and deactivated particles. VID Vector ID for DOF value of 4, see *DEFINE_VECTOR Remarks: Initially, the user defines the set of particles that are representing the flow of particles during the simulation. At time t = 0, all the particles are deactivated which means that no particle approximation is calculated. The boundary of activation is a plane determined by the NODE, and normal to the vector VID. The particles are activated when they reached the boundary. Since they are activated, particle approximation is started. *BOUNDARY_SPH_NON_REFLECTING Purpose: Define a non-reflecting boundary plane for SPH. This option applies to continuum domains modeled with SPH elements. Card 1 1 2 3 4 5 6 7 8 Variable VTX VTY VTZ VHX VHY VHZ Type F Default 0. F 0. F 0. F 0. F 0. F 0. VARIABLE DESCRIPTION x-coordinate of tail of a normal vector originating on the wall (tail) and terminating in the body (head) (i.e., vector points from the non-reflecting boundary plane into the body). y-coordinate of tail z-coordinate of tail x-coordinate of head y-coordinate of head z-coordinate of head VTX VTY VTZ VHX VHY VHZ Remarks: 1. The non-reflecting boundary plane has to be normal to either the x, y or z direction. *BOUNDARY_SPH_SYMMETRY_PLANE Purpose: Define a symmetry plane for SPH. This option applies to continuum domains modeled with SPH elements. Card 1 1 2 3 4 5 6 7 8 Variable VTX VTY VTZ VHX VHY VHZ Type F Default 0. F 0. F 0. F 0. F 0. F 0. VARIABLE DESCRIPTION x-coordinate of tail of a normal vector originating on the wall (tail) and terminating in the body (head) (i.e., vector points from the symmetry plane into the body). y-coordinate of tail z-coordinate of tail x-coordinate of head y-coordinate of head z-coordinate of head VTX VTY VTZ VHX VHY VHZ Remarks: 1. A plane of symmetry is assumed for all SPH elements defined in the model. 2. The plane of symmetry has to be normal to either the x, y or z direction. 3. For axi-symmetric SPH analysis, IDIM = -2, a plane of symmetry centered at the global origin and normal to x-direction is automatically created by LS-Dyna. *BOUNDARY_SYMMETRY_FAILURE Purpose: Define a symmetry plane with a failure criterion. This option applies to continuum domains modeled with solid elements. Card 1 1 Variable SSID Type I 2 FS F Default none 0. 3 4 5 6 7 8 VTX VTY VTZ VHX VHY VHZ F 0. F 0. F 0. F 0. F 0. F 0. VARIABLE DESCRIPTION Segment set ID, see *SET_SEGMENT Tensile failure stress > 0.0. The average stress in the elements surrounding the boundary nodes in a direction perpendicular to the boundary is used. x-coordinate of tail of a normal vector originating on the wall (tail) and terminating in the body (head) (i.e., vector points from the symmetry plane into the body). y-coordinate of tail z-coordinate of tail x-coordinate of head y-coordinate of head z-coordinate of head SSID FS VTX VTY VTZ VHX VHY VHZ Remarks: A plane of symmetry is assumed for the nodes on the boundary at the tail of the vector given above. Only the motion perpendicular to the symmetry plane is constrained. After failure the nodes are set free. *BOUNDARY_TEMPERATURE_OPTION Available options include: NODE SET Purpose: Define temperature boundary conditions for a thermal or coupled thermal/ structural analysis. Card 1 1 2 3 4 5 6 7 8 Variable NID/SID TLCID TMULT LOC Type I Default none I 0 F 0. I 0 VARIABLE DESCRIPTION NID/SID Node ID/Node Set ID, see *SET_NODE_OPTION TLCID Temperature, 𝑇, specification. This parameter can reference a load curve ID or a function ID . When the reference is to a curve, TLCID has the following interpretation: GT.0: 𝑇 is defined by a curve consisting of (𝑡, 𝑇) data pairs. EQ.0: 𝑇 is a constant defined by the value TMULT. TMULT Temperature, 𝑇, curve multiplier. LOC Application of surface for thermal shell elements, see parameter, THSHEL, in the *CONTROL_SHELL input: EQ.-1: lower surface of thermal shell element EQ.0: middle surface of thermal shell element EQ.1: upper surface of thermal shell element Remarks: 1. This keyword can be used to apply temperature boundary conditions to SPH particles. 2. If TLCID references a DEFINE_FUNCTION, the following function arguments are allowed 𝑓 (𝑥, 𝑦, 𝑧, 𝑣𝑥, 𝑣𝑦, 𝑣𝑧, 𝑡): 𝑥, 𝑦, 𝑧 = node point coordinates 𝑣𝑥, 𝑣𝑦, 𝑣𝑧 = node point velocity components 𝑡 = solution time *BOUNDARY_THERMAL_BULKFLOW_OPTION1_OPTION2 Purpose: Used to define bulk fluid flow elements. OPTION1 is required since it specifies whether the BULKFLOW applies to an element or set. ELEMENT SET OPTION2 if used turns on the fluid upwind algorithm UPWIND Card 1 1 2 3 4 5 6 7 8 Variable EID/SID LCID MDOT Type I I F Default none none none VARIABLE EID / SID DESCRIPTION Beam element ID (EID) for ELEMENT option Beam set ID (SID) for SET option LCID Load Curve ID for mass flow rate versus time. MDOT Mass flow rate (e.g. kg/sec). *BOUNDARY_THERMAL_BULKNODE Purpose: Used to define thermal bulk nodes. Card 1 1 2 3 4 5 Variable NID PID NBNSEG VOL LCID Type I I Default none none I 0 F none I 0 6 H F 0. 7 8 AEXP BEXP F 0. F 0. Bulk Node Cards. Include NBNSEG cards, one for each bulk node segment. Card 2 Variable 1 N1 Type I 2 N2 I 3 N3 I 4 N4 I 5 6 7 8 VARIABLE DESCRIPTION NID PID VOL Bulk node number. Bulk node part ID. Bulk node volume. NBNSEG Number of element surface segments that transfer heat with this bulk node. N1, N2, N3, N4 Nodal point numbers LCID H AEXP BEXP Load curve ID for H Heat transfer coefficient 𝑎 exponent 𝑏 exponent *BOUNDARY_THERMAL_BULKNODE The heat flow between a bulk node (TB) and a bulk node segment (TS) is given by 𝑞 = ℎ(𝑇𝐵 𝑎 − 𝑇𝐵 𝑎 )𝑏 1. For convection, set 𝑎 = 𝑏 = 1. 2. For radiation, set 𝑎 = 4, 𝑏 = 1. 3. For flux, set 𝑎 = 𝑏 = 0. Mathematically, anything to the 0 power is 1. This = (1 − 1)0 = 00 = 1. However, some com- to set It produces the expression, (𝑇𝐵 puter operating systems don’t 𝑎 = 𝑏 = very small number. recognize 00. 0) 0−𝑇𝑆 is safer *BOUNDARY_THERMAL_WELD Purpose: Define a moving heat source to model welding. Only applicable for a coupled thermal-structural simulations in which the weld source or work piece is moving. Card 1 1 2 3 4 Variable PID PTYP NID NFLAG Type I Default none Card 2 Variable Type 1 a F I 1 2 b F I none 3 cf F I 1 4 cr F 5 X0 F 6 Y0 F 7 Z0 F 8 N2ID I none none none none 5 LCID I 6 Q F 7 Ff F 8 Fr F Default none none none none none none none none Beam Aiming Direction Card. Additional card for N2ID = -1. 4 5 6 7 8 Optional Variable 1 TX Type F 2 TY F 3 TZ F Default none none none VARIABLE DESCRIPTION PID PTYP Part ID or Part Set ID to which weld source is applied PID type: EQ.1: PID defines a single part ID EQ.2: PID defines a part set ID Welding Torch velocity cr cf (a) (b) Figure 5-7. Schematic illustration of welding with moving torch. The left figure (a) shows the surface of the material from above, while the right figure (b) shows a slice along the dotted line in the y-z plane. VARIABLE DESCRIPTION NID Node ID giving location of weld source EQ.0: location defined by (X0, Y0, Z0) below NFLAG Flag controlling motion of weld source EQ.1: source moves with node NID EQ.2: source is fixed in space at original position of node NID X0, Y0, Z0 Coordinates of weld source, which remains fixed in space (optional, ignored if NID nonzero above) N2ID Second node ID for weld beam aiming direction GT.0: beam is aimed from N2ID to NID, moves with these nodes EQ.-1: beam aiming direction is (tx, ty, tz) input on optional card 3 a b cf cr Weld pool radius (i.e., half width) Weld pool depth (in beam aiming direction) Weld pool forward direction Weld pool rearward direction VARIABLE DESCRIPTION LCID Load curve ID for weld energy input rate vs. time EQ.0: use constant multiplier value Q. Q Ff Fr Curve multiplier for weld energy input rate [energy/time, e.g., Watt] LT.0: use absolute value and accurate integration of heat Forward distribution function Rear distribution function (Note:Ff + Fr = 2.0) TX, TY, TZ Weld beam direction vector in global coordinates (N2ID = -1 only) Remarks: This boundary condition allows simulation of a moving weld heat source, following the work of Goldak, Chakravarti, and Bibby [1984]. Heat is generated in an ellipsoidal region centered at the weld source, and decaying exponentially with distance according to: where: 𝑞 = 6√3𝐹𝑄 𝜋√𝜋𝑎𝑏𝑐 exp ( −3𝑥2 𝑎2 ) exp ( −3𝑦2 𝑏2 ) exp ( −3𝑧2 𝑐2 ) 𝑞 = weld source power density (𝑥, 𝑦, 𝑧) = coordinates of point 𝑝 in weld material 𝐹 = { 𝑐 = { Ff if point 𝑝 is in front of beam Fr if point 𝑝 is behind beam cf if point 𝑝 is in front of beam cr if point 𝑝 is behind beam A local coordinate system is constructed which is centered at the heat source. The relative velocity vector of the heat source defines the "forward" direction, so material points that are approaching the heat source are in "front" of the beam. The beam aiming direction is used to compute the weld pool depth. The weld pool width is measured normal to the relative velocity - aiming direction plane. If Q is defined negative in the input, then the formula above is using the absolute value of Q, and a more accurate integration of the heat source is performed with some additional cost in CPU time. To simulate a welding process during which the welding torch is fixed in space, NID and N2ID must be set to 0 and -1 respectively. The X0, Y0, and Z0 fields specify the global coordinates of the welding torch, and the TX, TY, and TZ fields specify the direction of the welding beam. The motion of the work piece is prescribed using the *BOUNDARY_PRESCRIBED_MOTION keyword. To simulate a welding process for which the work piece fixed in space, NID and N2ID specify both the beam source location and direction. The X0, Y0, Z0, TX, TY, and TZ fields are ignored. The motion of welding source is prescribed with using the *BOUND- ARY_PRESCRIBED_MOTION keyword applied to the two nodal points specified in the NID and N2ID fields. *BOUNDARY_THERMAL_WELD_TRAJECTORY Purpose: Define a moving heat source to model welding of solid or shell structures. Motion of the source is described by a nodal path and a prescribed velocity on this path. This keyword is applicable in coupled thermal-structural and thermal-only simulations and also supports thermal dumping. Different equivalent heat source descriptions are implemented. Card 1 1 2 3 4 5 6 7 8 Variable PID PTYP NSID1 VEL1 SID2 VEL2 NCYC RELVEL Type I Default none Card 2 1 I 1 2 Variable IFORM LCID Type I I I F I F none none none none 3 Q F 4 5 6 LCROT LCMOV LCLAT DISC I I I F I 1 7 Default none none none none none none none Card 3 Variable 1 P1 Type F 2 P2 F 3 P3 F 4 P4 F 5 P5 F 6 P6 F 7 P7 F I 0 8 8 P8 F Default none none none none none none none none Weld Source Aiming Direction Card. Additional card for NS2ID = 0. 4 5 6 7 8 Optional Variable 1 TX Type F 2 TY F 3 TZ F Default none none none VARIABLE PID DESCRIPTION Part ID or Part Set ID of solids or shells to which weld source is applied PTYP PID type: EQ.1: PID defines a single part ID EQ.2: PID defines a part set ID NSID1 Node set ID containing the path (weld trajectory) information for the weld source movement. A sorted node set is requested. The order defines the weld path and the direction . VEL1 Velocity of the heat source on the weld trajectory GT.0: constant velocity LT.0: |VEL1| is a load curve ID defining weld speed vs. time SID2 ID of second node set or segment set containing information for the weld source aiming direction GT.0: SID2 refers to a sorted node set, the order of which defines the direction of the trajectory. The heat source is aimed from current position in SID2 to current position in the weld trajectory. EQ.0: beam aiming direction is (tx, ty, tz) input on optional card 4. LT.0: |SID2| is a segment set. The heat source is aiming in normal direction to segments in the set. VARIABLE DESCRIPTION VEL2 Velocity of reference point in SID2, if SID2 > 0 GT.0: constant velocity LT.0: |VEL2| is a load curve ID defining weld speed vs. time NCYC RELVEL Number of substeps for subcycling in evaluation of boundary condition. Allows thermal dumping . Defines if VEL1 and VEL2 are relative or absolute velocities in coupled simulations EQ.0: absolute velocities EQ.1: relative velocities with respect to underlying structure IFORM Geometry description for energy rate density distribution : EQ.1: Goldak-type heat source EQ.2: double ellipsoidal heat source with constant density EQ.3: double conical heat source with constant density EQ.4: frustum-shaped heat source with constant density LCID Load curve ID for weld energy input rate vs. time EQ.0: use constant multiplier value Q. Q Curve multiplier for weld energy input rate [energy/time] LT.0: take absolute value and accurate integration of heat using integration cells with edge length DISC. LCROT LCMOV LCLAT DISC Load curve defining the rotation (angle in degree) of weld source around the trajectory as function of time . Load curve for offset of weld source in direction of the weld beam as function of time Load curve for lateral offset of weld source as function of time Resolution for accurate integration, parameter defines edge length for integration cubes. Default is 5% of weld pool depth. VARIABLE DESCRIPTION Pi Parameters defining for weld pool geometry, depending on parameter IFORM. See Remark 4 for details. TX, TY, TZ Weld beam direction vector in global coordinates (SID2 = 0 only) Remarks: 1.This keyword can be applied for solid and thermal thick shells in thermal-only and coupled thermal-structural simulations. The nodes in the node set NSID1 have to be ordered, such that the node set defines the path geometry as well as the direction of the trajectory. The heat source starts at the position of the first node in the node set and automatically ends as soon as the last node is reached. By choosing nodes of the work piece for the path definition in NSID1, it can be ensured that the heat source always follows the movement of the piece. By setting parameter RELVEL to 1 the velocity of the heat source can even be de- fined relatively to the motion of the structure. 2.If a segment set referred to in SID2 which coincides with the work piece surface, the weld beam direction is always orthogonal to the work piece surface. To be applicable every two consecutive nodes of node set NSID1 have to be part of at least one segment. In case of more than one segment an averaged normal is computed. Based on the trajectory and the weld source aiming direction, a local coordinate system is constructed that is centered at the root of the heat source. By default, the relative velocity vector (on the trajectory) of the heat source defines the "forward" direction 𝒓, so material points that are approaching the heat source are in "front" of the beam. The weld source aiming direction, denoted by 𝒕, is used to compute the weld pool depth. The weld pool width (coordinate direction 𝒔) is measured normal to the relative velocity - aiming direction plane. The keyword allows rotating and translating the coordinate system. First, the system is rotated around the vector 𝒓 by a value given in the load curve LCROT resulting in a new local coordinate system (𝒓, 𝒔′, 𝒕′). Second, the system is trans- lated in directions 𝒕′ and 𝒔′ using LCMOV and LCLAT, respectively. 3.The subcycling method introduces an individual time step size for the weld source evaluation. Within one time step of the heat transfer solver, NCYC steps are used to determine the energy rate distribution of the boundary condition. In each substep the geometry of the weld pool is updated. Therefore, even with larger thermal time steps a relatively smooth temperature field around the weld source can be obtained and a jumping heat source across elements can be sup- pressed. 4.This keyword allows application of different equivalent heat source geometries, depending on the parameter IFORM. The definition of the local coordinate system needed for the description of the weld pool shape is discussed in Remark 2. For IFORM.EQ.1 heat is generated in an ellipsoidal region centered at the weld source, and decaying exponentially with distance according to the work of Goldak, Chakravarti, and Bibby [1984]. Energy rate distribution is governed by 𝑞 = 2𝑛√𝑛𝐹𝑄 𝜋√𝜋𝑎𝑏𝑐 exp ( −𝑛𝑥2 𝑎2 ) exp ( −𝑛𝑦2 𝑏2 ) exp ( −𝑛𝑧2 𝑐2 ) where: 𝐹 = { 𝑐 = { Ff if point 𝑝 is in front of beam Fr if point 𝑝 is behind beam cf if point 𝑝 is in front of beam cr if point 𝑝 is behind beam The local coordinates of point 𝑝 are denoted by (𝑥, 𝑦, 𝑧) and it is expected that the sum of the weighting factors 𝐹f, 𝐹r equals 2. The half-width of the ellipsoid is given by 𝑎, the welding depth by 𝑏. The complete set of parameters (𝑎, 𝑏, 𝑐f, 𝑐r, 𝐹f, 𝐹r, 𝑛) is input by the parameters P1 to P7, see table below. The energy rate density 𝑞 defined by IFORM.EQ.2 is assumed to be constant in the double ellipsoidal region as defined for Goldak-type heat sources. Its value is given by 𝑞 = 3𝐹𝑄 2𝜋𝑎𝑏𝑐 with the same assumptions for 𝐹 and 𝑐 as above. The set of parameters conse- quently reduces to (𝑎, 𝑏, 𝑐f, 𝑐r, 𝐹f, 𝐹r), the input of which is given by P1 to P6. In contrast to the above IFORM.EQ.3 defines an equivalent heat source with a constant energy rate density on a double conical region. The shape is defined by three radii 𝑟1, 𝑟2, 𝑟3and two values 𝑏1, 𝑏2 defining the heights of the two parts of the shape. The respective power densities of the parts are given by 𝑞𝑖 = 3𝐹𝑖𝑄 2 + 𝑟𝑖+1 2𝜋𝑏𝑖(𝑟𝑖 2 + 𝑟𝑖 2 ) 2𝑟𝑖+1 . Here it is assumed that 𝑖 = 1 corresponds to the part closer to the weld source. The input for the complete parameter set (𝑟1, 𝑟2, 𝑟3, 𝑏1, 𝑏2, 𝐹1, 𝐹2) is again defined by P1 to P7. Finally, IFORM.EQ.4 defines a constant power density over a frustum. The density and the shape can easily be described using three geometrical parameters P1 to P3 corresponding to the radii 𝑟1(at the heat source origin) and 𝑟2 and the height 𝑏: 𝑞 = 1 𝑎 𝑏 𝑐f 𝑐r 𝐹f 𝐹r 𝑛 IFORM P1 P2 P3 P4 P5 P6 P7 P8 2 + 𝑟1 2 + 𝑟2 2) 2𝑟2 𝜋𝑏(𝑟1 4 𝑟1 𝑟2 𝑏1 2 𝑎 𝑏 𝑐f 𝑐r 𝐹f 𝐹r 3 𝑟1 𝑟2 𝑟3 𝑏1 𝑏2 𝐹f 𝐹r *BOUNDARY Purpose: Define a surface for coupling with the USA code [DeRuntz 1993]. The outward normal vectors should point into the fluid media. The coupling with USA is operational in explicit transient and in implicit natural frequency analyses. Card 1 2 3 4 5 6 7 8 Variable SSID WETDRY NBEAM Type I Default none I 0 I 0 VARIABLE DESCRIPTION SSID Segment set ID, see *SET_SEGMENT WETDRY Wet surface flag: EQ.0: Dry, no coupling for USA DAA analysis, or Internal fluid coupling for USA CASE analysis EQ.1: Wet, coupled with USA for DAA analysis, or External fluid coupling for USA CASE analysis The number of nodes touched by USA Surface-of-Revolution (SOR) elements. It is not necessary that the LS-DYNA model has beams where USA has beams (i.e., SOR elements), merely that the LS-DYNA model has nodes to receive the forces that USA will return. NBEAM Remarks: The underwater shock analysis code is an optional module. To determine availability contact sales@lstc.com. The wet surface of 3 and 4-noded USA general boundary elements is defined in LS- DYNA with a segment set of 4-noded surface segments, where the fourth node can duplicate the third node to form a triangle. The segment normal vectors should be directed into the USA fluid. If USA overlays are going to be used to reduce the size of the DAA matrices, the user should nonetheless define the wet surface here as if no overlay were being used. If Surface-of -Revolution elements (SORs) are being used in USA, then NBEAM should be non-zero on one and only one card in this section. The wet surface defined here can cover structural elements or acoustic fluid volume elements, but it can not touch both types in one model. When running a coupled problem with USA, the procedure requires an additional input file of USA keyword instructions. These are described in a separate USA manual. The name of this input file is identified on the command line with the usa = flag: where uin is the USA keyword instruction file. LSDYNA.USA i=inf usa=uin *BOUNDARY_ELEMENT_METHOD_OPTION Available options include: CONTROL FLOW NEIGHBOR SYMMETRY WAKE Purpose: incompressible fluid dynamics or fluid-structure interaction problems. Define input parameters for boundary element method analysis of The boundary element method (BEM) can be used to compute the steady state or transient fluid flow about a rigid or deformable body. The theory which underlies the method is restricted to inviscid, incompressible, attached fluid flow. The method should not be used to analyze flows where shocks or cavitation are present. In practice the method can be successfully applied to a wider class of fluid flow problems than the assumption of inviscid, incompressible, attached flow would imply. Many flows of practical engineering significance have large Reynolds numbers (above 1 million). For these flows the effects of fluid viscosity are small if the flow remains attached, and the assumption of zero viscosity may not be a significant limitation. Flow separation does not necessarily invalidate the analysis. If well-defined separation lines exist on the body, then wakes can be attached to these separation lines and reasonable results can be obtained. The Prandtl-Glauert rule can be used to correct for non-zero Mach numbers in a gas, so the effects of aerodynamic compressibility can be correctly modeled (as long as no shocks are present). The BOUNDARY_ELEMENT_METHOD_FLOW card turns on the analysis, and is mandatory. *BOUNDARY_ELEMENT_METHOD_CONTROL Purpose: Control the execution time of the boundary element method calculation. The CONTROL option is used to control the execution time of the boundary element method calculation, and the use of this option is strongly recommended. The BEM calculations can easily dominate the total execution time of a LS-DYNA run unless the parameters on this card (especially DTBEM and/or IUPBEM) are used appropriately. DTBEM is used to increase the time increment between calls to the BEM routines. This can usually be done with little loss in accuracy since the characteristic times of the structural dynamics and the fluid flow can differ by several orders of magnitude. The characteristic time of the structural dynamics in LS-DYNA is given by the size of the smallest structural element divided by the speed of sound of its material. For a typical problem this characteristic time might be equal to 1 microsecond. Since the fluid in the boundary element method is assumed to be incompressible (infinite speed of sound), the characteristic time of the fluid flow is given by the streamwise length of the smallest surface in the flow divided by the fluid velocity. For a typical problem this characteristic time might be equal to 10 milliseconds. For this example DTBEM might be set to 1 millisecond with little loss of accuracy. Thus, for this example, the boundary element method would be called only once for every 1000 LS-DYNA iterations, saving an enormous amount of computer time. IUPBEM is used to increase the number of times the BEM routines are called before the matrix of influence coefficients is recomputed and factored (these are time-consuming procedures). If the motion of the body is entirely rigid body motion there is no need to ever recompute and factor the matrix of influence coefficients after initialization, and the execution time of the BEM can be significantly reduced by setting IUPBEM to a very large number. For situations where the structural deformations are modest an intermediate value (e.g., 10) for IUPBEM can be used. Card 1 1 2 3 4 5 6 7 8 Variable LWAKE DTBEM IUPBEM FARBEM Type I Default 50 F 0. I F 100 2.0 Remark 1 DESCRIPTION Number of elements in the wake of lifting surfaces. Wakes must be defined for all lifting surfaces. Time increment between calls to the boundary element method. The fluid pressures computed during the previous call to the BEM will continue to be used for subsequent LS-DYNA iterations until a time increment of DTBEM has elapsed. The number of times the BEM routines are called before the matrix of influence coefficients is recomputed and refactored. Nondimensional boundary between near-field and far-field calculation of influence coefficients. VARIABLE LWAKE DTBEM IUPBEM FARBEM Remarks: 1. Wakes convect with the free-stream velocity. The number of elements in the wake should be set to provide a total wake length equal to 5-10 times the char- acteristic streamwise length of the lifting surface to which the wake is attached. Note that each wake element has a streamwise length equal to the magnitude of the free stream velocity multiplied by the time increment between calls to the boundary element method routines. This time increment is controlled by DTBEM. 2. The most accurate results will be obtained with FARBEM set to 5 or more, while values as low as 2 will provide slightly reduced accuracy with a 50% reduction in the time required to compute the matrix of influence coefficients. *BOUNDARY_ELEMENT_METHOD_FLOW Purpose: Turn on the boundary element method calculation, specify the set of shells which define the surface of the bodies of interest, and specify the onset flow. The *BOUNDARY_ELEMENT_METHOD_FLOW card turns on the BEM calculation. This card also identifies the shell elements which define the surfaces of the bodies of interest, and the properties of the onset fluid flow. The onset flow can be zero for bodies which move through a fluid which is initially at rest. Card 1 1 Variable SSID Type I 2 VX F 3 VY F 4 VZ F 5 6 7 8 RO PSTATIC MACH F F Default none none none none none 0. Remark 1 2 F 0. 3 VARIABLE SSID DESCRIPTION Shell set ID for the set of shell elements which define the surface of the bodies of interest . The nodes of these shells should be ordered so that the shell normals point into the fluid. VX, VY, VZ x, y, and z components of the free-stream fluid velocity. RO Fluid density. PSTATIC Fluid static pressure. MACH Free-stream Mach number. Remarks: 1. It is recommended that the shell segments in the SSID set use the NULL material . This will provide for the display of fluid pressures in the post-processor. For triangular shells the 4th node number should be the same as the 3rd node number. For fluid-structure interaction problems it is recommended that the boundary element shells use the same nodes and be coincident with the structural shell elements (or the outer face of solid ele- ments) which define the surface of the body. This approach guarantees that the boundary element segments will move with the surface of the body as it de- forms. 2. A pressure of PSTATIC is applied uniformly to all segments in the segment set. If the body of interest is hollow, then PSTATIC should be set to the free-stream static pressure minus the pressure on the inside of the body. 3. The effects of subsonic compressibility on gas flows can be included using a non-zero value for MACH. The pressures which arise from the fluid flow are increased using the Prandtl-Glauert compressibility correction. MACH should be set to zero for water or other liquid flows. *BOUNDARY_ELEMENT_METHOD_NEIGHBOR Purpose: Define the neighboring elements for a given boundary element segment. The pressure at the surface of a body is determined by the gradient of the doublet distribution on the surface . The “Neighbor Array” is used to specify how the gradient is computed for each boundary element segment. Ordinarily, the Neighbor Array is set up automatically by LS-DYNA, and no user input is required. The NEIGHBOR option is provided for those circumstances when the user desires to define this array manually. Elements Cards. The next “*” card terminates the input. Card 1 1 2 3 4 5 6 7 8 Variable NELEM NABOR1 NABOR2 NABOR3 NABOR4 Type I I I I I Default none none none none none VARIABLE DESCRIPTION NELEM Element number. NABOR1 Neighbor for side 1 of NELEM. NABOR2 Neighbor for side 2 of NELEM. NABOR3 Neighbor for side 3 of NELEM. NABOR4 Neighbor for side 4 of NELEM. Remarks: Each boundary element has 4 sides (Figure 6-1). Side 1 connects the 1st and 2nd nodes, side 2 connects the 2nd and 3rd nodes, etc. The 4th side is null for triangular elements. node 4 side 3 node 3 side 4 node 1 segment(j) side 1 side 2 node 2 Figure 6-1. Each segment has 4 sides. For most elements the specification of neighbors is straightforward. For the typical case a quadrilateral element is surrounded by 4 other elements, and the neighbor array is as shown in Figure 6-2. neighbor(3, j) side 3 neighbor(4, j) side 4 segment(j) side 1 side 2 neighbor(2, j) neighbor(1, j) Figure 6-2. Typical neighbor specification. There are several situations for which the user may desire to directly specify the neighbor array for certain elements. For example, boundary element wakes result in discontinuous doublet distributions, and neighbors which cross a wake should not be used. Figure 6-3 illustrates a situation where a wake is attached to side 2 of segment j. For this situation two options exist. If neighbor(2,j) is set to zero, then a linear computation of the gradient in the side 2 to side 4 direction will be made using the difference between the doublet strengths on segment j and segment neighbor(4,j). This is the default setup used by LS-DYNA when no user input is provided. By specifying neighbor(2,j) as a negative number a more accurate quadratic curve fit will be used to compute the gradient. The curve fit will use segment j, segment neighbor(4,j), and segment -neighbor(2,j); which is located on the opposite side of segment neighbor(4,j) as segment j. -neighbor(2, j) neighbor(4, j) side 3 side 4 segment(j) side 1 side 2 Figure 6-3. If neighbor(2,j) is a negative number it is assumed to lie on the opposite side of neighbor(4,j) as segment j. Another possibility is that no neighbors at all are available in the side 2 to side 4 direction. In this case both neighbor(2,j) and neighbor(4,j) can be set to zero, and the gradient in that direction will be assumed to be zero. This option should be used with caution, as the resulting fluid pressures will not be accurate for three-dimensional flows. However, this option is occasionally useful where quasi-two dimensional results are desired. All of the above options apply to the side 1 to side 3 direction in the obvious ways. For triangular boundary elements side 4 is null. Gradients in the side 2 to side 4 direction can be computed as described above by setting neighbor(4,j) to zero for a linear derivative computation (this is the default setup used by LS-DYNA when no user input is provided) or to a negative number to use the segment on the other side of neighbor(2,j) and a quadratic curve fit. There may also be another triangular segment which can be used as neighbor(4,j) . neighbor(4, j) segment(j) side 2 Figure 6-4. Sometimes another triangular boundary element segment can be used as neighbor (4,j). The rules for computing the doublet gradient in the side 2 to side 4 direction can be summarized as follows (the side 1 to side 3 case is similar): NABOR2 NABOR4 Doublet Gradient Computation GT.0 GT.0 Quadratic fit using elements j, NABOR2, and NABOR4. LT.0 GT.0 GT.0 LT.0 Quadratic fit using elements j, -NAB- OR2, and NABOR4. -NABOR2 is assumed to lie on the opposite side of NABOR4 as segment j . Quadratic fit using elements j, NABOR2, and -NABOR4. -NABOR4 is assumed to lie on the opposite side of NABOR2 as segment j. EQ.0 GT.0 GT.0 EQ.0 EQ.0 EQ.0 Linear fit using elements j and NABOR4. Linear fit using elements j and NABOR2. Zero gradient. Table 3.1 Surface pressure computation for element j. *BOUNDARY_ELEMENT_METHOD_SYMMETRY Purpose: To define a plane of symmetry for the boundary element method. The SYMMETRY option can be used to reduce the time and memory required for symmetric configurations. For these configurations the reduction in the number of boundary elements by a factor of 2 will reduce the memory used by the boundary element method by a factor of 4, and will reduce the computer time required to factor the matrix of influence coefficients by a factor of 8. Only 1 plane of symmetry can be defined. Card 1 1 2 3 4 5 6 7 8 Variable BEMSYM Type Default I 0 VARIABLE DESCRIPTION BEMSYM Defines symmetry plane for boundary element method. EQ.0: no symmetry plane is defined EQ.1: x = 0 is a symmetry plane EQ.2: y = 0 is a symmetry plane EQ.3: z = 0 is a symmetry plane *BOUNDARY_ELEMENT_METHOD_WAKE Purpose: To attach wakes to the trailing edges of lifting surfaces. Wakes should be attached to boundary elements at the trailing edge of a lifting surface (such as a wing, propeller blade, rudder, or diving plane). Wakes should also be attached to known separation lines when detached flow is known to exist (such as the sharp leading edge of a delta wing at high angles of attack). Wakes are required for the correct computation of surface pressures for these situations. As described above, two segments on opposite sides of a wake should never be used as neighbors. Element Cards. (The next “*” card terminates the input.) Card 1 1 2 3 4 5 6 7 8 Variable NELEM NSIDE Type I I Default none none Remark 1 VARIABLE DESCRIPTION NELEM Element number to which a wake is attached. NSIDE The side of NELEM to which the wake is attached . This should be the "downstream" side of NELEM. Remarks: 1. Normally two elements meet at a trailing edge (one on the "upper" surface and one on the "lower" surface). The wake can be attached to either element, but not to both. The *CASE command provides a way of running multiple LS-DYNA analyses (or cases) sequentially by submitting a single input file. When *CASE commands are used to define multiple cases, some portions of the input will be shared by some or all of the cases and other portions will be unique to each case. Because the cases are run sequentially, the results from one case, e.g., a dynain file, can be used in the analysis of a different, subsequent case. Each case creates a unique set of output file names by prepending “casen.” to the default file name, e.g., case101.d3plot, case102.glstat. When the *CASE keyword appears in an input deck, it becomes necessary to append the word “CASE” to the LS-DYNA execution line. For example, an SMP LS-DYNA execution line might look something like path_to_ls-dyna i=input.k ncpu=-4 CASE An MPP LS-DYNA execution line might look something like mpirun –np 4 path_to_mpp971 i=input.k CASE *CASE_{OPTION} Available options include: <BLANK> BEGIN_N END_N Purpose: Define a series of cases and perhaps subcases. The options *CASE_BEGIN_n and *CASE_END_n appear in pairs and n is a numeric ID of a subcase. Subcase IDs may be referenced by the *CASE command in defining a case. In other words, a case may consist of one or more subcases. All keywords appearing between *CASE_BE- GIN_n and *CASE_END_n comprise subcase n. If no *CASE command is defined, then subcases defined by *CASE_BEGIN_n and *CASE_END_n then become cases. *CASE_- BEGIN/*CASE_END can be nested, overlapped, and disjointed. Examples below demonstrate the use of these options. An alternative way of defining subcases is by appending the string “CID = n” to the end of any keyword command. Any keyword so tagged will then be active only for those cases that reference subcase n. There can be more than one space between the keyword and “CID = n”. Any keyword in the input deck not associated with a subcase is active for all cases. GIN/*CASE_END. Card 1 1 2 3 4 5 6 7 8 Variable CASEID JOBID Type I C Default none none Command Line Argument Cards. Command line cards set additional command line arguments for the case CASEID . Include as many as needed, or as few as none. Command line cards end when the first character of the next card is numeric. Card 2 1 2 3 4 5 6 7 8 Variable Type Default COMMANDS A Not Required Subcase ID Cards. Define active subcase IDs for case CASEID . These cards continue until the next keyword (“*”) card. Card 3 1 2 Variable SCID1 SCID2 Type I I 3 … I 4 … I 5 … I 6 … I 7 … I 8 … I Default none none none none none none none none VARIABLE DESCRIPTION CASEID Identification number for case. VARIABLE JOBID DESCRIPTION Optional string (no spaces) to be used as the jobid for this case. If no JOBID is specified, the string CASEXX is used, where XX is the CASEID in field 1 *CASE COMMANDS Command line arguments. SCIDn Subcase ID active for case CASEID. Remarks: 1. 2. 3. If no *CASE keyword appears, subcases defined with *CASE_BEGIN/*CASE_- END commands become cases and *CASE_BEGIN can optionally be followed by extra command line arguments. If no *CASE keyword appears, it is an error to append “CID = n” to any keyword. If multiple *CASE or *CASE_BEGIN keywords appear that have the same ID, their command line arguments and active commands are merged. 4. The *CASE or *CASE_BEGIN keywords cannot be used within an include (*IN- CLUDE) file. Example 1: $$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ $ $ Define case 101 which includes subcase 1. $ Define case 102 which includes subcase 4. $$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ $ *CASE $ $...>....1....>....2....>....3....>....4....>....5....>....6....>....7 $ CASEID 101 JOBID_FOR_CASE101 MEMORY=20M 1 $ *CASE $ CASEID 102 MEMORY=20M NCYCLE=1845 4 $ *TITLE CID=1 THIS IS THE TITLE FOR CASE 101 $ *TITLE CID=4 THIS IS THE TITLE FOR CASE 102 $$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ $ $$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ $ $$$$ Illustrate overlapping subcases. $ $$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ $ *CASE_BEGIN_5 $...>....1....>....2....>....3....>....4....>....5....>....6....>....7....> *DATABASE_BINARY_D3THDT 1.e-5 *CASE_BEGIN_3 *DATABASE_NODOUT 1.e-5 *CASE_END_5 *DATABASE_ELOUT 1.e-5 *CASE_END_3 $ $$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ Example 2 above will generate d3thdt and nodout for CID = 5, and nodout and elout for CID = 3. *COMMENT All input that falls between a *COMMENT command and the subsequent line of input that has an asterisk in the first column thereby signaling the start of another keyword command, is not acted on by LS-DYNA. This provides a convenient way to interject multiple, successive lines of commentary anywhere inside an input deck. *COMMENT also provides a convenient way to comment out an exisiting keyword command and all its associated input data as shown in an example below. Lines of input that are deactivated by *COMMENT are echoed on the screen and to the messag and d3hsp files. Card 1 1 2 3 4 5 6 7 8 Variable Type Default COMMENT A none VARIABLE DESCRIPTION COMMENT Any comment line. Example: In this excerpt from an input deck, 5 lines of comments including blank lines, are added to the input deck. *KEYWORD *COMMENT Units of this model are mks. Input prepared by John Doe. Input checked by Jane Doe. *CONTROL_TERMINATION 1.E-02 ⋮ *COMMENT In this excerpt from an input deck, a contact is disabled by inserting *COMMENT command before the contact keyword command. ⋮ *COMMENT *CONTACT_AUTOMATIC_SURFACE_TO_SURFACE_ID $# cid title 1 $# ssid msid sstyp mstyp sboxid mboxid spr mpr 1,2,0,3 $# fs fd dc vc vdc penchk bt dt 0.2 $# sfs sfm sst mst sfst sfmt fsf vsf $# soft sofscl lcidab maxpar sbopt depth bsort frcfrq 2 *SET_SEGMENT $# sid da1 da2 da3 da4 solver 1 0.000 0.000 0.000 0.000MECH $# n1 n2 n3 n4 a1 a2 a3 a4 2842 626 3232 3242 0.000 0.000 0.000 0.000 2846 2842 627 2843 0.000 0.000 0.000 0.000 ⋮ The keyword *COMPONENT provides a way of incorporating specialized components and features. The keyword control cards in this section are defined in alphabetical order: *COMPONENT_GEBOD_OPTION *COMPONENT_GEBOD_JOINT_OPTION *COMPONENT_HYBRIDIII *COMPONENT_HYBRIDIII_JOINT_OPTION *COMPONENT_GEBOD Purpose: Generate a rigid body dummy based on dimensions and mass properties from the GEBOD database. The motion of the dummy is governed by equations integrated within LS-DYNA separately from the finite element model. Default joint characteristics (stiffness’s, stop angles, etc.) are set internally and should give reasonable results, however, they may be altered using the *COMPONENT_GEBOD_- JOINT command. Contact between the segments of the dummy and the finite element model is defined using the *CONTACT_GEBOD command. The use of a positioning file is essential with this feature, see Appendix N for further details. OPTION specifies the human subject type. The male and female types represent adults while the child is genderless. MALE FEMALE CHILD Card 1 1 2 3 4 5 6 7 8 Variable DID UNITS SIZE Type I I F Default none none none Card 2 Variable 1 VX Type F Default 0. 2 VY F 0. 3 VZ F 0. 4 GX F 0. 5 GY F 0. 6 GZ F 0. 7 8 VARIABLE DESCRIPTION DID Dummy ID. A unique number must be specified. VARIABLE DESCRIPTION UNITS System of units used in the finite element model. EQ.1: lbf × sec2/in - inch - sec EQ.2: kg - meter - sec EQ.3: kgf × sec2/mm - mm - sec EQ.4: metric ton - mm - sec EQ.5: kg - mm - msec SIZE Size of the dummy. This represents a combined height and weight percentile ranging from 0 to 100 for the male and female types. For the child the number of months of age is input with an admissible range from 24 to 240. VX, VY, VZ Initial velocity of the dummy in the global x, y and z directions. GX, GY, GZ Global x, y, and z components of gravitational acceleration applied to the dummy. Example: $$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ $ $$$$ *COMPONENT_GEBOD_MALE $ $$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ $ $ A 50th percentile male dummy with the ID number of 7 is generated in the $ lbf*sec^2-inch-sec system of units. The dummy is given an initial velocity of $ 616 in/sec in the negative x direction and gravity acts in the negative z $ direction with a value 386 in/sec^2. $ *COMPONENT_GEBOD_MALE $ $...>....1....>....2....>....3....>....4....>....5....>....6....>....7....>....8 $ did units size 7 1 50 $ vx vy vz gx gy gz -616 0 0 0 0 -386 $ $$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ $ *COMPONENT_GEBOD_JOINT_OPTION Purpose: Alter the joint characteristics of a GEBOD rigid body dummy. Setting a joint parameter value to zero retains the default value set internally. See Appendix N for further details. The following options are available. PELVIS WAIST LOWER_NECK UPPER_NECK LEFT_SHOULDER RIGHT_SHOULDER LEFT_ELBOW RIGHT_ELBOW LEFT_HIP RIGHT_HIP LEFT_KNEE RIGHT_KNEE LEFT_ANKLE RIGHT_ANKLE Card 1 1 2 3 4 5 6 7 8 Variable DID LC1 LC2 LC3 SCF1 SCF2 SCF3 Type F I I I F F F VARIABLE DESCRIPTION DID LCi SCFi Dummy ID, see *COMPONENT_GEBOD_OPTION. Load curve ID specifying the loading torque versus rotation (in radians) for the ith degree of freedom of the joint. Scale factor applied to the load curve of the ith joint degree of freedom. Card 2 Variable 1 C1 Type F 2 C2 F 3 C3 F 4 5 6 7 8 NEUT1 NEUT2 NEUT3 F F F VARIABLE DESCRIPTION Ci Linear viscous damping coefficient applied to the ith DOF of the joint. Units are torque × time/radian, where the units of torque and time depend on the choice of UNITS in card 1 of *COMPO- NENT_GEBOD_OPTION. NEUTi Neutral angle (degrees) of joint's ith DOF. Card 3 1 2 3 4 5 6 7 8 Variable LOSA1 HISA1 LOSA2 HISA2 LOSA3 HISA3 Type F F F F F F VARIABLE DESCRIPTION LOSAi HISAi Value of the low stop angle (degrees) for the ith DOF of this joint. Value of the high stop angle (degrees) for the ith DOF of this joint. Card 4 1 2 3 4 5 6 7 8 Variable UNK1 UNK2 UNK3 Type F Default 0. F 0. F 0. DESCRIPTION Unloading stiffness (torque/radian) for the ith degree of freedom of the joint. This must be a positive number. Units of torque depend on the choice of UNITS in card 1 of *COMPONENT_GE- BOD_OPTION. VARIABLE UNKi Example 1: $$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ $ $$$$ *COMPONENT_GEBOD_JOINT_LEFT_SHOULDER $ $$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ $ $ The damping coefficients applied to all three degrees of freedom of the left $ shoulder of dummy 7 are set to 2.5. All other characteristics of this joint $ remain set to the default value. $ *COMPONENT_GEBOD_JOINT_LEFT_SHOULDER $ $...>....1....>....2....>....3....>....4....>....5....>....6....>....7....>....8 $ did lc1 lc2 lc3 scf1 scf2 scf3 7 0 0 0 0 0 0 $ c1 c2 c3 neut1 neut2 neut3 2.5 2.5 2.5 0 0 0 $ losa1 hisa1 losa2 hisa2 losa3 hisa3 0 0 0 0 0 0 $ unk1 unk2 unk3 0 0 0 $ $$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ Example 2: $$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ $ $$$$ *COMPONENT_GEBOD_JOINT_WAIST $ $$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ $ $ Load curve 8 gives the torque versus rotation relationship for the 2nd DOF $ (lateral flexion) of the waist of dummy 7. Also, the high stop angle of the $ 1st DOF (forward flexion) is set to 45 degrees. All other characteristics $ of this joint remain set to the default value. $ *COMPONENT_GEBOD_JOINT_WAIST $ $...>....1....>....2....>....3....>....4....>....5....>....6....>....7....>....8 $ did lc1 lc2 lc3 scf1 scf2 scf3 7 0 8 0 0 0 0 $ c1 c2 c3 neut1 neut2 neut3 0 0 0 0 0 0 $ losa1 hisa1 losa2 hisa2 losa3 hisa3 0 45 0 0 0 0 $ unk1 unk2 unk3 0 0 0 $ $$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ *COMPONENT_HYBRIDIII Purpose: Define a HYBRID III dummy. The motion of the dummy is governed by equations integrated within LS-DYNA separately from the finite element model. The dummy interacts with the finite element structure through contact interfaces. Joint characteristics (stiffnesses, damping, friction, etc.) are set internally and should give reasonable results, however, they may be altered using the *COMPONENT_HYBRIDI- II_JOINT command. Joint force and moments can be written to an ASCII file . Card 1 1 2 3 4 Variable DID SIZE UNITS DEFRM Type I I I Default none none none I 1 8 5 VX F 0. 6 VY F 0. 7 VZ F 0. VARIABLE DESCRIPTION DID SIZE Dummy ID. A unique number must be specified. Size of dummy. EQ.1: 5th percentile adult EQ.2: 50th percentile adult EQ.3: 95th percentile adult NOTE: If negative then the best of currently available joint properties are applied. UNITS System of units used in the finite element model. EQ.1: lbf × sec2/in - inch - sec EQ.2: kg - meter - sec EQ.3: kgf × sec2/mm - mm - sec EQ.4: metric ton - mm - sec EQ.5: kg - mm - msec VARIABLE DESCRIPTION DEFRM Deformability type. EQ.1: all dummy segments entirely rigid EQ.2: deformable abdomen (low density foam, mat #57) EQ.3: deformable jacket (low density foam, mat #57) EQ.4: deformable headskin (viscoelastic, mat #6) EQ.5: deformable abdomen/jacket EQ.6: deformable jacket/headskin EQ.7: deformable abdomen/headskin EQ.8: deformable abdomen/jacket/headskin VX, VY, VZ Initial velocity of the dummy in the global x, y and z directions. Card 2 Variable 1 HX Type F Default 0. 2 HY F 0. 3 HZ F 0. 4 RX F 0. 5 RY F 0. 6 RZ F 0. 7 8 VARIABLE DESCRIPTION HX, HY, HZ Initial global x, y, and z coordinate values of the H-point. RX, RY, RZ Initial rotation of dummy about the H-point with respect to the global x, y, and z axes (degrees). Example 1: $$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ $ $$$$ *COMPONENT_HYBRIDIII $ $$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ $ $ A 50th percentile adult rigid HYBRID III dummy with an ID number of 7 is defined $ in the lbf*sec^2-inch-sec system of units. The dummy is assigned an initial $ velocity of 616 in/sec in the negative x direction. The H-point is initially $ situated at (x,y,z)=(38,20,0) and the dummy is rotated 18 degrees about the $ global x-axis. $ *COMPONENT_HYBRIDIII $ $...>....1....>....2....>....3....>....4....>....5....>....6....>....7....>....8 $ did . size units defrm vx vy vz 7 2 1 1 -616. 0. 0. $ hx hy hz rx ry rz 38. 20. 0. 18. 0. 0. $ $$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ *COMPONENT_HYBRIDIII_JOINT_OPTION Purpose: Alter the joint characteristics of a HYBRID III dummy. Setting a joint parameter value to zero retains the default value set internally. Joint force and moments can be written to an ASCII file . Further details pertaining to the joints are found in the Hybrid III Dummies section of Appendix N. The following options are available: LUMBAR RIGHT_ELBOW RIGHT_KNEE LOWER_NECK LEFT_WRIST LEFT_ANKLE UPPER_NECK RIGHT_WRIST RIGHT_ANKLE LEFT_SHOULDER LEFT_HIP STERNUM RIGHT_SHOULDER RIGHT_HIP LEFT_KNEE_SLIDER LEFT_ELBOW LEFT_KNEE RIGHT_KNEE_SLIDER Card 1 1 Variable DID Type F Card 2 Variable 1 C1 2 Q1 F 2 3 Q2 F 3 4 Q3 F 4 5 6 7 8 FRIC F 5 6 7 8 ALO1 BLO1 AHI1 BHI1 QLO1 QHI1 SCLK1 Type F F F F F F F F Leave blank if joint has only one degree of freedom. Card 3 Variable 1 C2 2 3 4 5 6 7 8 ALO2 BLO2 AHI2 BHI2 QLO2 QHI2 SCLK2 Type F F F F F F F Leave blank if the joint has only two degrees of freedom. Card 4 Variable 1 C3 2 3 4 5 6 7 8 ALO3 BLO3 AHI3 BHI3 QLO3 QHI3 SCLK3 Type F F F F F F F F VARIABLE DESCRIPTION Dummy ID, see *COMPONENT_HYBRIDIII Initial value of the joint's ith degree of freedom. Units of degrees are defined for rotational DOF. See Appendix N for a listing of the applicable DOF. Friction load on the joint. Linear viscous damping coefficient applied to the ith DOF of the joint. Linear coefficient for the low regime spring of the joint's ith DOF. Cubic coefficient for the low regime spring of the joint's ith DOF. Linear coefficient for the high regime spring of the joint's ith DOF. Cubic coefficient for the high regime spring of the joint's ith DOF. Value at which the low regime spring definition becomes active. Value at which the high regime spring definition becomes active. Scale value applied to the stiffness of the (default = 1.0). joint's ith DOF DID Qi FRIC Ci ALOi BLOi AHIi BHIi QLOi QHIi SCLKi Example: $$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ $ $$$$ *COMPONENT_HYBRIDIII_JOINT_LEFT_ANKLE $ $$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ $ $ The damping coefficients applied to all three degrees of freedom of the left $ ankle of dummy 7 are set to 2.5. All other characteristics of this joint $ remain set to the default value. The dorsi-plantar flexion angle is set to $ 20 degrees. $ *COMPONENT_HYBRIDIII_JOINT_LEFT_ANKLE $ $...>....1....>....2....>....3....>....4....>....5....>....6....>....7....>....8 $ did q1 q2 q3 fric 7 0 20. 0 0 0 $ c1 alo1 blo1 ahi1 bhi1 qlo1 qhi1 2.5 0 0 0 0 0 0 $ c2 alo2 blo2 ahi2 bhi2 qlo2 qhi2 2.5 0 0 0 0 0 0 $ 2.5 alo3 blo3 ahi3 bhi3 qlo3 qhi3 The keyword *CONSTRAINED provides a way of constraining degrees of freedom to move together in some way. The keyword cards in this section are defined in alphabetical order: *CONSTRAINED_ADAPTIVITY *CONSTRAINED_BEAM_IN_SOLID *CONSTRAINED_BUTT_WELD *CONSTRAINED_COORDINATE_{OPTION} *CONSTRAINED_EULER_IN_EULER *CONSTRAINED_EXTRA_NODES_OPTION *CONSTRAINED_GENERALIZED_WELD_OPTION_{OPTION} *CONSTRAINED_GLOBAL *CONSTRAINED_INTERPOLATION_{OPTION} *CONSTRAINED_INTERPOLATION_SPOTWELD *CONSTRAINED_JOINT_OPTION_{OPTION}_{OPTION}_{OPTION} *CONSTRAINED_JOINT_COOR_OPTION_{OPTION}_{OPTION}_{OPTION} *CONSTRAINED_JOINT_STIFFNESS_OPTION *CONSTRAINED_JOINT_USER_FORCE *CONSTRAINED_LAGRANGE_IN_SOLID *CONSTRAINED_LINEAR_GLOBAL *CONSTRAINED_LINEAR_LOCAL *CONSTRAINED_LOCAL *CONSTRAINED_MULTIPLE_GLOBAL *CONSTRAINED_NODAL_RIGID_BODY_{OPTION}_{OPTION} *CONSTRAINED_NODE_INTERPOLATION *CONSTRAINED_NODE_TO_NURBS_PATCH *CONSTRAINED_POINTS *CONSTRAINED_RIGID_BODIES *CONSTRAINED_RIGID_BODY_INSERT *CONSTRAINED_RIGID_BODY_STOPPERS *CONSTRAINED_RIVET_{OPTION} *CONSTRAINED_SHELL_TO_SOLID *CONSTRAINED_SPLINE *CONSTRAINED_SPOTWELD_{OPTION}_{OPTION} *CONSTRAINED_SPR2 *CONSTRAINED_TIEBREAK *CONSTRAINED_TIED_NODES_FAILURE *CONSTRAINED_ADAPTIVITY Purpose: Constrains a node to the midpoint along an edge of an element. This keyword is automatically created by LS-DYNA during an h-adaptive simulation involving 3-D shells. Card 1 Variable 1 SN 2 3 4 5 6 7 8 MN1 MN2 Type I I I Default none none none VARIABLE DESCRIPTION SN MN1 MN2 Slave node. This is the node constrained at the midpoint of an edge of an element. The node at one end of an element edge. The node at the other end of that same element edge. *CONSTRAINED_BEAM_IN_SOLID_{OPTION} Available options include: <BLANK> ID TITLE Purpose: This keyword constrains beam structures to move with Lagrangian solids/thick shells, which serve as the master component. This keyword constrains both acceleration and velocity. This feature is intended to sidestep certain limitations in the CTYPE = 2 implementation in *CONSTRAINED_LAGRANGE_IN_SOLID. Notable features of this keyword include: 1. CDIR = 1 feature. With the CDIR = 1 option coupling occurs only in the normal directions. This coupling allows for releasing the constraints along beam axial direction. 2. Axial coupling force. Debonding processes can be modeled with a user defined function or user provided subroutine giving the axial shear force based on the slip between rebar nodes and concrete solid elements. This feature is invoked by setting AXFOR flag to a negative integer which refers to the *DE- FINE_FUNCTION ID or a number greater than 1000. In the latter case, first we need to modify the subroutine rebar_bondslip_get_getforce() in dyn21.F to add in one or more debonding laws; each tagged with a “lawid”. Then we could specify which debonding law to use with the AXFOR flag. AXFOR value great- er than 1000 will call the user subroutine and pass AXFOR in as “lawid”. CDIR has to be set to 1 in this case to release the axial constraints. 3. NCOUP feature. Coupling not only at nodes, but also at multiple coupling points in between the two beam element nodes. Please note, the previous im- plementation done in *CONSTRAINED_LAGRANGE_IN_SOLID CTYPE 2 causes errors in energy balance. 4. Tetrahedral and pentahedra solid elements are supported. They are treated as degenerated hexahedra in CTYPE2 implementation. 5. Velocity/Fixed boundary condition. The CTYPE 2 implementation failed to constrain beam nodes that were buried inside elements whose nodes had veloc- ity/fixed boundary conditions prescribed. 6. Optimized Sorting. Sorting subroutine is optimized for larger problems to achieve better performance and less memory usage. If a title is not defined, LS-DYNA will automatically create an internal title for this coupling definition. Title Card. Additional card for TITLE and ID keyword options. Title 1 2 3 4 5 6 7 8 Variable COUPID Type I TITLE A70 Card 1 1 2 3 4 5 6 7 8 Variable SLAVE MASTER SSTYP MSTYP NCOUP CDIR I 0 7 I 0 8 5 6 Type I I Default none none Card 2 1 2 I 0 3 I 0 4 Variable START END AXFOR Type Default F 0 F 1010 I 0 VARIABLE COUPID DESCRIPTION Coupling (card) ID number (I10). If not defined, LS-DYNA will assign an internal coupling ID based on the order of appearance in the input deck. TITLE A description of this coupling definition. SLAVE Slave set ID defining a part, part set ID of the Lagrangian beam structure . VARIABLE MASTER DESCRIPTION Master set ID defining a part or part set ID of the Lagrangian solid elements or thick shell elements . SSTYP Slave set type of “SLAVE”: EQ.0: part set ID (PSID). EQ.1: part ID (PID). MSTYP Master set type of “MASTER”: EQ.0: part set ID (PSID). EQ.1: part ID (PID). NCOUP Number of coupling points generated in one beam element. If set to 0, coupling only happens at beam nodes. Otherwise, coupling is done at both the beam nodes and those automatically generated coupling points. CDIR Coupling direction. EQ.0: default, constraint applied along all directions. EQ.1: Constraint only applied along normal directions; along the beam axial direction there is no constraint. START Start time for coupling. END End time for coupling. AXFOR ID of a user defined function describes coupling force versus slip along beam axial direction. GE.0: EQ.-n: OFF n is the function ID in *DEFINE_FUNCTION EQ.n > 1000: n is the debonding law id “lawid” in user defined subroutine rebar_bondslip_get_force(). Example: 1. The example below shows how to define a function and use it to prescribe the debonding process. User can define his own function based on different debonding theories. $...|....1....|....2....|....3....|....4....|....5....|....6....|....7....|... .8 *CONSTRAINED_BEAM_IN_SOLID $# slave master sstyp mstyp ctype empty nquad idir 2 1 1 1 0 2 1 $# start end axfor 0.000 0.000 -10 *DEFINE_FUNCTION 10 float force(float slip,float leng) { float force,pi,d,area,shear,pf; pi = 3.1415926; d = 0.175; area = pi*d*leng; pf = 1.0; if (slip < 0.25) { shear = slip*pf; } else { shear = 0.25*pf; } force = shear*area; return force; } $...|....1....|....2....|....3....|....4....|....5....|....6....|....7....|... .8 2. The example below shows how to define a user subroutine and use it to prescribe the debonding process. $...|....1....|....2....|....3....|....4....|....5....|....6....|....7....|... .8 *CONSTRAINED_BEAM_IN_SOLID $# slave master sstyp mstyp ctype empty nquad idir 2 1 1 1 0 2 1 $# start end axfor 0.000 0.000 1001 *CONSTRAINED_BEAM_IN_SOLID $# slave master sstyp mstyp ctype empty nquad idir 3 1 1 1 0 2 1 $# start end axfor 0.000 0.000 1002 *USER_LOADING $ parm1 parm2 parm3 parm4 parm5 parm6 parm7 parm8 1.0 6.0 $...|....1....|....2....|....3....|....4....|....5....|....6....|....7....|... .8 And the user debonding law subroutine: subroutine rebar_bondslip_get_force(slip,dl,force,hsv, . userparm,lawid) real hsv dimension hsv(12),cm(8),userparm(*) c c in this subroutine user defines debonding properties and c call his own debonding subroutine to get force cm(1)=userparm(1) cm(2)=userparm(2) cm(3)=2.4*(cm(2)/5.0)**0.75 cm(8)=0. c pi = 3.1415926 d = 0.175 area = pi*0.25*d*d*dl pf = 1.0 c if (lawid.eq.1001) then if (slip.lt.0.25) then shear = slip*pf else shear = 0.25*pf endif force = sign(1.0,slip)*shear*area elseif (lawid.eq.1002) then if (slip.lt.0.125) then shear = slip*pf else shear = 0.125*pf endif endif return end *CONSTRAINED_BUTT_WELD Purpose: Define a line of coincident nodes that represent a structural butt weld between two parts defined by shell elements. Failure is based on nodal plastic strain for ductile failure and stress resultants for brittle failure. This input is much simpler than the alternative approach for defining butt welds, see *CONSTRAINED_GENERAL- IZED_WELD_BUTT. The local coordinate system, the effective length, and thickness for each pair of butt welded nodes are determined automatically in the definition below. In the GENERALIZED option these quantities must be defined in the input. Card 1 1 2 3 4 5 6 7 8 Variable SNSID MNSID EPPF SIGF BETA Type I I F F F Default none none 0. 1.e+16 1.0 Remarks 1, 2 3, 4 3 3 VARIABLE DESCRIPTION SNSID Slave node set ID, see *SET_NODE_OPTION. MNSID Master node set ID, see *SET_NODE_OPTION. EPPF SIGF Plastic strain at failure 𝜎𝑓 , stress at failure for brittle failure. BETA 𝛽, failure parameter for brittle failure. Remarks: 1. Nodes in the master and slave sets must be given in the order they appear as one moves along the edge of the surface. An equal number of coincident nodes must be defined in each set. In a line weld the first and last node in a string of nodes can be repeated in the two sets. If the first and last pair of nodal points are identical, a circular or closed loop butt weld is assumed. See Figure 10-1, where the line butt weld and closed loop weld are illustrated. local y-axis Length of butt weld Repeated nodal point may start or end a butt weld line. This beginning or ending nodal point must exist in both and slave and master definitions Two coincident butt welded nodal points. Repeated nodal point pair must start and end circular butt weld. Any nodal pair in the circle can be used. Figure 10-1. Definition of butt welds are shown above. The butt weld can be represented by a line of nodal points or by a closed loop 2. Butt welds may not cross. For complicated welds, this option can be combined with the input in *CONSTRAINED_GENERALIZED_WELD_BUTT to handle the case where crossing occurs. Nodes in a butt weld must not be members of rigid bodies. 3. If the average volume-weighted effective plastic strain in the shell elements adjacent to a node exceeds the specified plastic strain at failure, the node is released. Brittle failure of the butt welds occurs when: 𝛽√𝜎𝑛 2 + 3(𝜏𝑛 2 + 𝜏𝑡 2) ≥ 𝜎𝑓 where, 𝜎𝑛 = normal stress (local x) 𝜏𝑛 = shear stress in direction of weld (local y) 𝜏𝑡 = shear stress normal to weld (local z) 𝜎𝑓 = failure stress 𝛽 = failure parameter The component σn is nonzero for tensile values only. The nodes defining the slave and master sides of the butt weld must coincide. The local z-axis at a master node is normal to the master side plane of the butt weld at the node, and the local y-axis is taken as the vector in the direction of a line connecting the mid-points of the line segments lying on either side of the master node. The normal vector is found by summing the unit normal vectors of all shell ele- ments on the master side sharing the butt welded node. The direction of the normal vector at the node is chosen so that the x-local vector points towards the elements on the slave side in order to identify tensile versus compressive stresses. The thickness of the butt weld and length of the butt weld are needed to compute the stress values. The thickness is based on the average thickness of the shell elements that share the butt welded nodal pair, and the chosen length of the butt weld is shown in Figure 10-1. 4. Butt welds may be used to simulate the effect of failure along a predetermined line, such as a seam or structural joint. When the failure criterion is reached at a nodal pair, the nodes begin to separate. As this effect propagates, the weld will appear to “unzip,” thus simulating failure of the connection. *CONSTRAINED_COORDINATE_{OPTION} To define constraints based on position coordinates the following options are available: <BLANK> LOCAL Purpose: The keyword is developed to allow the definition of constraints in position coordinates in springback simulation. With the frequent application of adaptive mesh in stamping simulation, nodes needed for springback constraints are often unavailable until the last process simulation before springback is complete. On the other hand, if the nodes are available, their positions may not be exactly on the desired locations required for springback constraints. With this new keyword, the springback simulation is no longer dependent on the previous process simulation results and the exact springback constraint locations can be specified. Card 1 Variable 1 ID 2 3 PID IDIR Type I I I 4 X1 F 5 Y1 F 6 Z1 F Default none none none 0.0 0.0 0.0 8 7 CID I 0 VARIABLE DESCRIPTION ID PID IDIR Identification number of a constraint. Part ID of the part to be constrained. Applicable degrees-of-freedom being constrained: EQ.1: x translational degree-of-freedom, EQ.2: y translational degree-of-freedom, EQ.3: z translational degree-of-freedom. X1, Y1, Z1 X, Y, Z coordinates of the location being constrained. CID Local coordinate system ID. Figure 10-2. Constrained locations of a trim panel (NUMISHEET 2005 cross member). General remarks: The identification number of a constraint must be unique; in particular, the IDs must be unique even for two constraints involving the same X, Y, Z coordinates but different degrees of freedom. When the LOCAL option is invoked, a local coordinate system ID, as defined with *DEFINE_COORDINATE_{OPTION} keyword, should be provided in the CID field. Defining constraints using coordinates can now be done in Springback process of LS- PrePost4.0 eZSetup for metal forming application, using the Pick location button (http://- ftp.lstc.com/anonymous/outgoing/lsprepost/4.0/metalforming/). Application example: An example of using the keyword is listed below. A part with PID 18 is constrained in 6 locations in a local coordinate system ID 9, defined by the keyword *DEFINE_COOR- DINATE_SYSTEM. Constrained DOFs are indicated by IDIR. $---+----1----+----2----+----3----+----4----+----5----+----6----+----7----+----8 *CONSTRAINED_COORDINATE $ ID IDPT IDIR x y z CID 1 18 2 -555.128 86.6 1072.29 9 2 18 3 -555.128 86.6 1072.29 9 3 18 3 -580.334 -62.15 1068.32 9 4 18 1 568.881 81.2945 1033.72 9 5 18 2 568.881 81.2945 1033.72 9 6 18 3 568.881 81.2945 1033.74 9 ) ( - ) ( - 150 100 50 -50 -100 SPC Force @ Nodes A B C D E F G H I J 0.2 0.4 0.6 0.8 Time (Sec.) Figure 10-3. SPC Z-forces at 10 nodes. 140 120 100 80 60 40 20 SPC Force @ Nodes Sum SPC force 10 nodes 0.2 0.4 0.6 0.8 Time (Sec.) Figure 10-4. SPC Z-force summation of the 10 nodes *DEFINE_COORDINATE_SYSTEM $ CID X0 Y0 Z0 XL YL ZL 9 0.0 0.0 0.0 0.0 10.0 0.0 $ XP YP ZP 10.0 10.0 0.0 It is possible to output SPC forces on the coordinates constrained. For each position coordinate set, an extra node will be generated and SPC forces are calculated and output to SPCFORC file. The frequency of the output is specified with the keyword *DATABASE_SPCFORC. Shown in the Figure 10-2 are the Z-constrained locations on the trimmed panel (half with symmetric conditions at the smaller end) of the NUMISHEET 2005 cross member. SPC forces in Z direction of these 10 locations were recovered after a multi-steps static implicit springback with this over-constrained boundary condition, Figure 10-3. The summation of these Z-forces is shown in Figure 10-4 and it approaches to zero as the residual stresses are balanced out by the springback shape, absent of gravity. Revision information: This feature is now available in LS-DYNA R5 Revision 52619 or later releases. The SPC output feature is available in LS-DYNA Revision 62560 and later releases, both in SMP and MPP. *CONSTRAINED_EULER_IN_EULER Purpose: This command defines the coupling interaction between EULERIAN materials in two overlapping, geometrically similar, multi-material Eulerian mesh sets. The command allows a frictionless “contact” between two or more different Eulerian materials. Card 1 1 2 3 4 5 6 7 8 Variable PSIDSLV PSIDMST PFAC Type Default I 0 I 0 F 0.1 VARIABLE DESCRIPTION PSIDSLV Part set ID of the 1st ALE or Eulerian set of mesh(es) (slave). PSIDMST Part set ID of the 2nd ALE or Eulerian set of mesh(es) (master). PFAC A penalty factor for the coupling interaction between the two PSIDs. Remarks: 1. The 2 meshes must be of Eulerian formulation (the meshes are fixed in space, not moving). Consider 2 overlapping Eulerian meshes. Each Eulerian mesh contains 2 physical materials, say a vacuum and a metal. This card provides a frictionless “contact” or interaction between the 2 metals, each resides in a dif- ferent Eulerian mesh system. Due to its restrictive nature, this option is cur- rently only an experimental feature. 2. Contact pressure is built up in two overlapping Eulerian elements if their combined material fill fraction exceeds 1.0 (penalty formulation). 3. This feature needs to be combined with *MAT_VACUUM (element formula- tion 11). Example: Consider an ALE/Eulerian multi-material model (ELFORM = 11) consisting of: PID 1 = *MAT_NULL (material 1) PID 2 = *MAT_VACUUM ⇒ PID 1 is merged at its boundary to PID 2. PID 3 = *MAT_NULL (material 3) PID 4 = *MAT_VACUUM ⇒ PID 3 is merged at its boundary to PID 4. The mesh set containing PID 1 & 2 intersects or overlaps with the mesh set containing PID 3 & 4. PID 1 is given an initial velocity in the positive x direction. This will cause material 1 to contact material 3 (note that materials 2 & 4 are void). The interaction between materials 1 & 3 is possible by defining this coupling command. In this case material 1 can flow within the mesh region of PID 1 & 2 only, and material 3 can flow within the mesh region of PID 3 & 4 only. $...|....1....|....2....|....3....|....4....|....5....|....6....|....7....|...8 *ALE_MULTI-MATERIAL_GROUP $ SID SIDYTPE 1 1 2 1 3 1 4 1 *CONSTRAINED_EULER_IN_EULER $ PSID1 PSID2 PENAL 11 12 0.1 *SET_PART_LIST 11 1 2 *SET_PART_LIST 12 3 4 $...|....1....|....2....|....3....|....4....|....5....|....6....|....7....|...8 *CONSTRAINED_EXTRA_NODES_OPTION Available options include: NODE SET Purpose: Define extra nodes for rigid body. Card 1 1 2 3 4 5 6 7 8 Variable PID NID/NSID IFLAG Type I I Default none none I 0 VARIABLE PID DESCRIPTION Part ID of rigid body to which the nodes will be added, see *PART. NID / NSID Node (keyword option: NODE) or node set ID (keyword option: SET), see *SET_NODE, of added nodes. This flag is meaningful if and only if the inertia properties of the Part ID are defined in PART_INERTIA. If set to unity, the center- of-gravity, the translational mass, and the inertia matrix of the PID will be updated to reflect the merged nodal masses of the node or node set. If IFLAG is defaulted to zero, the merged nodes will not affect the properties defined in PART_INERTIA since it is assumed the properties already account for merged nodes. IFLAG Remarks: Extra nodes for rigid bodies may be placed anywhere, even outside the body, and they are assumed to be part of the rigid body. They have many uses including: 1. The definition of draw beads in metal forming applications by listing nodes along the draw bead. 2. Placing nodes where joints will be attached between rigid bodies. 3. Defining a node where point loads are to be applied or where springs may be attached. 4. Defining a lumped mass at a particular location. The coordinates of the extra nodes are updated according to the rigid body motion. Examples: $$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ $ $$$$ *CONSTRAINED_EXTRA_NODES_NODE $ $$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ $ $ Rigidly attach nodes 285 and 4576 to part 14. (Part 14 MUST be a rigid body.) $ *CONSTRAINED_EXTRA_NODES_NODE $ $...>....1....>....2....>....3....>....4....>....5....>....6....>....7....>....8 $ pid nid 14 285 14 4576 $ $$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ $ $ $$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ $ $$$$ *CONSTRAINED_EXTRA_NODES_SET $ $$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ $ $ Rigidly attach all nodes in set 4 to part 17. (Part 17 MUST be a rigid body.) $ $ In this example, four nodes from a deformable body are attached $ to rigid body 17 as a means of joining the two parts. $ *CONSTRAINED_EXTRA_NODES_SET $ $...>....1....>....2....>....3....>....4....>....5....>....6....>....7....>....8 $ pid nsid 17 4 $ $ *SET_NODE_LIST $ sid 4 $ nid1 nid2 nid3 nid4 nid5 nid6 nid7 nid8 665 778 896 827 $ $ $$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ $ *CONSTRAINED_GENERALIZED_WELD_OPTION_{OPTION} Available options include: SPOT FILLET BUTT CROSS_FILLET COMBINED To define an ID for the weld use the option: ID Purpose: Define spot, fillet, butt, and other types of welds. Coincident nodes are permitted if the local coordinate ID is defined. For the spot weld a local coordinate ID is not required if the nodes are offset. Failures can include both the plastic and brittle failures. These can be used either independently or together. Failure occurs when either criteria is met. The welds may undergo large rotations since the equations of rigid body mechanics are used to update their motion. Weld constraints between solid element nodes are not supported. ID Card. Additional card for ID keyword option. ID Card 1 2 3 4 5 6 7 8 Variable WID Type Default I Card 1 1 2 3 4 5 6 7 8 Variable NSID CID FILTER WINDOW NPR NPRT Type I I I E I I Default none none VARIABLE DESCRIPTION WID NSID CID FILTER WINDOW Optional weld ID. Nodal set ID, see *SET_NODE_OPTION. Coordinate system ID for output of spot weld data to SWFORC in local system, see *DEFINE_COORDINATE_OPTION. CID is not required for spot welds if the nodes are not coincident. Number of force vectors saved for filtering. This option can eliminate spurious failures due to numerical force spikes; however, memory requirements are significant since 6 force components are stored with each vector. LE.1: no filtering GE.2: simple average of force components divided by FILTER or the maximum number of force vectors that are stored for the time window option below. Time window for filtering. This option requires the specification of the maximum number of steps which can occur within the filtering time window. If the time step decreases too far, then the filtering time window will be ignored and the simple average is used. EQ.0: time window is not used NPR Number of individual nodal pairs in the cross fillet or combined general weld. VARIABLE DESCRIPTION NPRT Print option in file rbdout. EQ.0: default from the control card, *CONTROL_OUTPUT, is used, see variable name IPRTF. EQ.1: data is printed EQ.2: data is not printed Spot Weld Card. Additional Card required SPOT keyword option. Card 2 1 2 Variable TFAIL EPSF Type F F 3 SN F 4 SS F 5 N F 6 M F 7 8 VARIABLE DESCRIPTION TFAIL Failure time for constraint set, tf . (default = 1.E+20) Effective plastic strain at failure, 𝜖fail 𝑝 defines ductile failure. Sn, normal force at failure, only for the brittle failure of spot welds. Ss, shear force at failure, only for the brittle failure of spot welds. n, exponent for normal force, only for the brittle failure of spot welds. m, exponent for shear force, only for the brittle failure of spot welds. EPSF SN SS N M Remarks: Spot weld failure due to plastic straining occurs when the effective nodal plastic strain 𝑝 . This option can model the tearing out of a spot weld from exceeds the input value, 𝜀fail the sheet metal since the plasticity is in the material that surrounds the spot weld, not the spot weld itself. A least squares algorithm is used to generate the nodal values of plastic strains at the nodes from the element integration point values. The plastic strain is integrated through the element and the average value is projected to the nodes via a node 3 node 2 node 1 node 2 node 1 2 NODE SPOTWELD xx node N node N - 1 N NODE SPOTWELD node 2 node 1 Figure 10-5. Nodal ordering and orientation of the local coordinate system is important for determining spotweld failure. least square fit. This option should only be used for the material models related to metallic plasticity and can result in slightly increased run times. Brittle failure of the spot welds occurs when: [ max(𝑓𝑛, 0) 𝑆𝑛 ] + [ ∣𝑓𝑠∣ 𝑆𝑠 ] ≥ 1 where fn and fs are the normal and shear interface force. Component fn contributes for tensile values only. When the failure time, tf, is reached the nodal rigid body becomes inactive and the constrained nodes may move freely. In Figure 10-5 the ordering of the nodes is shown for the 2 node and 3 node spot welds. This order is with respect to the local coordinate system where the local z-axis determines the tensile direction. The nodes in the spot weld may coincide. The failure of the 3 node spot weld may occur gradually with first one node failing and later the second node may fail. For n noded spot welds the failure is progressive starting with the outer nodes (1 and n) and then moving inward to nodes 2 and n - 1. Progressive failure is necessary to preclude failures that would create new rigid bodies. Fillet Weld Card. Additional Card required for the FILLET keyword option. Card 2 1 2 3 4 Variable TFAIL EPSF SIGF BETA Type F F F F 5 L F 6 W F 7 A F 8 ALPHA F VARIABLE DESCRIPTION TFAIL Failure time for constraint set, tf (default = 1.E+20). EPSF SIGF Effective plastic strain at failure, 𝜖fail 𝑝 defines ductile failure. 𝜎𝑓 , stress at failure for brittle failure. BETA 𝛽, failure parameter for brittle failure. L W A L, length of fillet weld . w, separation of parallel fillet welds . a, fillet weld throat dimension . ALPHA 𝛼, weld angle in degrees. Remarks: Ductile fillet weld failure, due to plastic straining, is treated identically to spot weld failure. Brittle failure occurs when the following weld stress condition is met on the narrowest fillet weld cross section (across the throat): 𝛽√𝜎𝑛 2 + 3(𝜏𝑛 2 + 𝜏𝑡 2) ≥ 𝜎𝑓 Where 𝜎𝑛 = normal stress 𝜏𝑛 = shear stress in local z-x plane 𝜏𝑡 = 𝑠hear stress in local-y direction 2 Node Fillet Weld local coordinate system 3 Node Fillet Weld Figure 10-6. Nodal ordering and orientation of the local coordinate system is shown for fillet weld failure. The angle is defined in degrees. 𝜎𝑓 = failure stress 𝛽 = failure parameter The component 𝜎𝑛 is nonzero for tensile values only. When the failure time, 𝑡𝑓 , is reached the nodal rigid body becomes inactive and the constrained nodes may move freely. In Figure 10-6 the ordering of the nodes is shown for the 2 node and 3 node fillet welds. This order is with respect to the local coordinate system where the local z axis determines the tensile direction. The initial orientation of the local coordinate system is defined by CID. If CID = 0 then the global coordinate system is used. The local coordinate system is updated according to the rotation of the rigid body representing the weld. The failure of the 3 node fillet weld may occur gradually with first one node failing and later the second node may fail. LL 11 22 11 22 22 11 22 11 22 11 22 11 22 11 22 2 tied nodes that can be coincident Figure 10-7. Orientation of the local coordinate system and nodal ordering is shown for butt weld failure. Butt Weld Card. Additional Card required for the BUTT keyword option. Card 2 1 2 3 4 Variable TFAIL EPSF SIGY BETA Type F F F F 5 L F 6 D F 8 VARIABLE DESCRIPTION TFAIL Failure time for constraint set, tf . (default = 1.E+20) EPSF SIGY Effective plastic strain at failure, 𝜖fail 𝑝 defines ductile failure. 𝜎𝑓 , stress at failure for brittle failure. BETA 𝛽, failure parameter for brittle failure. L, length of butt weld . d, thickness of butt weld . L D Remarks: Ductile butt weld failure, due to plastic straining, is treated identically to spot weld failure. Brittle failure of the butt welds occurs when: 𝛽√𝜎𝑛 2 + 3(𝜏𝑛 2 + 𝜏𝑡 2) ≥ 𝜎𝑓 where 𝜎𝑛 = normal stress 𝜏𝑛 = shear stress in direction of weld (local y) 𝜏𝑡 = shear stress normal to weld (local z) 𝜎𝑓 = failure stress 𝛽 = failure parameter The component σn is nonzero for tensile values only. When the failure time, tf , is reached the nodal rigid body becomes inactive and the constrained nodes may move freely. The nodes in the butt weld may coincide. Example: $$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ $ $$$$ *CONSTRAINED_GENERALIZED_WELD_BUTT $ $$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ $ $ Weld two plates that butt up against each other at three nodal pair $ locations. The nodal pairs are 32-33, 34-35 and 36-37. $ $ This requires 3 separate *CONSTRAINED_GENERALIZED_WELD_BUTT definitions, $ one for each nodal pair. Each weld is to have a length (L) = 10, $ thickness (D) = 2, and a transverse length (Lt) = 1. $ $ Failure is defined two ways: $ Ductile failure if effective plastic strain exceeds 0.3 $ Brittle failure if the stress failure criteria exceeds 0.25 $ - scale the brittle failure criteria by beta = 0.9. $ Note: beta > 1 weakens weld beta < 1 strengthens weld $ *CONSTRAINED_GENERALIZED_WELD_BUTT $ $...>....1....>....2....>....3....>....4....>....5....>....6....>....7....>....8 $ nsid cid 21 $ tfail epsf sigy beta L D Lt 0.3 0.250 0.9 10.0 2.0 1.0 $ $ *CONSTRAINED_GENERALIZED_WELD_BUTT $ nsid cid 23 $ tfail epsf sigy beta L D Lt 0.3 0.250 0.9 10.0 2.0 1.0 $ $ *CONSTRAINED_GENERALIZED_WELD_BUTT $ nsid cid 25 $ tfail epsf sigy beta L D Lt 0.3 0.250 0.9 10.0 2.0 1.0 $ $ *SET_NODE_LIST $ sid 21 $ nid1 nid2 32 33 *SET_NODE_LIST 23 34 35 *SET_NODE_LIST 25 36 37 $ $$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ Cross Fillet Weld Card. Additional Card for the CROSS_FILLET keyword option. Card 2 1 2 3 4 Variable TFAIL EPSF SIGY BETA Type F F F F 5 L F 6 W F 7 A F 8 ALPHA F Nodal Pair Cards. Read NPR additional cards for the CROSS_FILLET keyword option. Card 3 1 2 3 4 5 6 7 8 Variable NODEA NODEB NCID Type I I I VARIABLE DESCRIPTION TFAIL Failure time for constraint set, tf . (default = 1.E+20) EPSF SIGY Effective plastic strain at failure, 𝜖fail 𝑝 defines ductile failure. 𝜎𝑓 , stress at failure for brittle failure. BETA 𝛽, failure parameter for brittle failure. L W A L, length of fillet weld . w, separation of parallel fillet welds . a, throat dimension of fillet weld . ALPHA 𝛼, weld angle in degrees. y2 (a) z1 y1 x1 z2 x2 (c) (b) y3 x3 z3 (d) Figure 10-8. A simple cross fillet weld illustrates the required input. Here NPR = 3 with nodal pairs (A = 2, B = 1), (A = 3, B = 1), and (A = 3, B = 2). The local coordinate axes are shown. These axes are fixed in the rigid body and are referenced to the local rigid body coordinate system which tracks the rigid body rotation. VARIABLE NODEA DESCRIPTION Node ID, A, in weld pair (CROSS or COMBINED option only). See Figure 10-8. VARIABLE DESCRIPTION NODEB Node ID, B, in weld pair (CROSS or COMBINED option only). NCID Local coordinate system ID (CROSS or COMBINED option only). Combined Weld Cards: Additional cards for the COMBINED keyword option. Read in NPR pairs of Cards 2 and 3 for a total of 2 × NPR cards. Card 2 1 2 3 4 Variable TFAIL EPSF SIGY BETA Type F Card 3 1 F 2 F 3 F 4 Variable NODEA NODEB NCID WTYP Type I I I I 5 L F 5 6 W F 6 7 A F 7 8 ALPHA F 8 VARIABLE DESCRIPTION TFAIL Failure time for constraint set, tf . (default = 1.E+20) EPSF SIGY Effective plastic strain at failure, 𝜖fail 𝑝 defines ductile failure. 𝜎𝑓 , stress at failure for brittle failure. BETA 𝛽, failure parameter for brittle failure. L W A L, length of fillet/butt weld . w, width of flange . a, width of fillet weld . ALPHA 𝛼, weld angle in degrees. 3 node Fillet Butt Weld Figure 10-9. A combined weld is a mixture of fillet and butt welds. VARIABLE DESCRIPTION NODEA Node ID, A, in weld pair (CROSS or COMBINED option only). NODEB Node ID, B, in weld pair (CROSS or COMBINED option only). NCID Local coordinate system ID (CROSS or COMBINED option only). WTYPE Weld pair type (GENERAL option only). See Figure 10-9. EQ.0: fillet weld EQ.1: butt weld *CONSTRAINED_GLOBAL 7 8 Purpose: Define a global boundary constraint plane. Card 1 Variable Type Default 1 TC I 0 2 RC I 0 3 DIR I 0 4 X F 0 5 Y F 0 6 Z F 0 VARIABLE DESCRIPTION TC Translational Constraint: EQ.1: constrained x translation, EQ.2: constrained y translation, EQ.3: constrained z translation, EQ.4: constrained x and y translations, EQ.5: constrained y and z translations, EQ.6: constrained x and z translations, EQ.7: constrained x, y, and z translations, RC Rotational Constraint: EQ.1: constrained x-rotation, EQ.2: constrained y-rotation, EQ.3: constrained z-rotation, EQ.4: constrained x and y rotations, EQ.5: constrained y and z rotations, EQ.6: constrained z and x rotations, EQ.7: constrained x, y, and z rotations. VARIABLE DESCRIPTION DIR Direction of normal for constraint plane. EQ.1: global x, EQ.2: global y, EQ.3: global z. X Y Z Global x-coordinate of a point on the constraint plane. Global y-coordinate of a point on the constraint plane. Global z-coordinate of a point on the constraint plane. Remarks: Nodes within a mesh-size-dependent tolerance are constrained on a global plane. This option is recommended for use with r-method adaptive remeshing where nodal constraints are lost during the remeshing phase. See *CONSTRAINED_LOCAL for specifying constraints to nodes lying on a local plane. *CONSTRAINED_INTERPOLATION_{OPTION} Available options include: <BLANK> LOCAL Purpose: Define an interpolation constraint. With this constraint type, the motion of a single dependent node is interpolated from the motion of a set of independent nodes. This option is useful for the redistribution of a load applied to the dependent node by the surrounding independent nodes. This load may be a translational force or a rotational moment. This keyword is typically used to model shell-brick and beam-brick interfaces. The mass and rotary inertia of the dependent nodal point is also redistributed. This constraint is applied in the global coordinate system unless the option LOCAL is active. One *CONSTRAINED_INTERPOLATION card is required for each constraint definition. The input list of independent nodes is terminated when the next "*" card is found. In explicit calculations the independent nodes cannot be dependent nodes in other constraints such as nodal rigid bodies; however, implicit calculations are not bound by this limitation. Card 1 1 2 3 4 5 6 7 8 Variable ICID DNID DDOF CIDD ITYP Type Default I 0 I I I 0 123456 optional I Independent Node Card Sets: If LOCAL option is not set, for each independent node include the following card; if the LOCAL keyword option is set, include only the following pair of cards. This input is terminated at the next keyword (“*”) card. Card 2 1 2 3 4 5 6 7 8 Variable INID IDOF TWGHTX TWGHTY TWGHTZ RWGHTX RWGHTY RWGHTZ Type I I F F F F F F Default 0 123456 1.0 TWGHTX TWGHTX TWGHTX TWGHTX TWGHTX Local Coordinate Card. Additional card for the LOCAL keyword option to be paired with card 2. Card 3 1 2 3 4 5 6 7 8 Variable CIDI Type Default I 0 VARIABLE DESCRIPTION ICID DNID DDOF Interpolation constraint ID. Dependent node ID. This node should not be a member of a rigid body, or elsewhere constrained in the input. Dependent degrees-of-freedom. The list of dependent degrees-of- freedom consists of a number with up to six digits, with each digit representing a degree of freedom. For example, the value 1356 indicates that degrees of freedom 1, 3, 5, and 6 are controlled by the constraint. The default is 123456. Digit: degree of freedom ID's: EQ.1: x EQ.2: y VARIABLE DESCRIPTION EQ.3: z EQ.4: rotation about x axis EQ.5: rotation about y axis EQ.6: rotation about z axis CIDD Local coordinate system ID if LOCAL option is active. If blank the global coordinate system is assumed. ITYP Specifies the meaning of INID. EQ.0: INID is a node ID EQ.1: INID is a node set ID Independent node ID or node set ID. Independent degrees-of-freedom using the same form as for the dependent degrees-of-freedom, DDOF, above. Weighting factor for node INID with active degrees-of-freedom IDOF. This weight scales the x-translational component. It is normally sufficient to define only TWGHTX even if its degree-of- freedom is inactive since the other factors are set equal to this input value as the default. There is no requirement on the values that are chosen as the weighting factors, i.e., that they sum to unity. The default value for the weighting factor is unity. Weighting factor for node INID with active degrees-of-freedom IDOF. This weight scales the y-translational component. Weighting factor for node INID with active degrees-of-freedom IDOF. This weight scales the z-translational component. Weighting factor for node INID with active degrees-of-freedom IDOF. This weight scales the x-rotational component. Weighting factor for node INID with active degrees-of-freedom IDOF. This weight scales the y-rotational component. Weighting factor for node INID with active degrees-of-freedom IDOF. This weight scales the z-rotational component. INID IDOF TWGHTX TWGHTY TWGHTZ RWGHTX RWGHTY RWGHTZ CIDI Local coordinate system ID if LOCAL option is active. If blank the global coordinate system is assumed. 21 22 11 45 44 33 43 Figure 10-10. Illustration of Example 1. Example 1: $$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ $ $$$$ *CONSTRAINED_INTERPOLATION (Beam to solid coupling) $ $$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ $ $ Tie a beam element to a solid element. $ $ The node of the beam to be tied does not share a common node with the solids. $ If the beam node is shared, for example, then set ddof=456. $ *CONSTRAINED_INTERPOLATION $ $...>....1....>....2....>....3....>....4....>....5....>....6....>....7....>....8 $ icid dnid ddof 1 45 123456 $ inid idof twghtx twghty twghtz rwghtx rwghty rwghtz 22 123 44 123 43 123 $ *......... $ 180 179 178 177 100 99 98 97 96 Figure 10-11. Illustration of Example 2. Example 2: $$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ $ $$$$ *CONSTRAINED_INTERPOLATION (Load redistribution) $ $$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ $ $ Moment about normal axis of node 100 is converted to an equivalent load by $ applying x-force resultants to the nodes lying along the right boundary $ *DEFINE_CURVE 1,0,0.,0.,0.,0.,0 0.,0. .1,10000. *LOAD_NODE_POINT 100,6,1,1.0 $ *CONSTRAINED_INTERPOLATION $ $...>....1....>....2....>....3....>....4....>....5....>....6....>....7....>....8 $ icid dnid ddof 1 100 5 $ inid idof twghtx twghty twghtz rwghtx rwghty rwghtz 96 1 97 1 98 1 99 1 177 1 178 1 179 1 180 1 $ *......... $ *CONSTRAINED_INTERPOLATION_SPOTWELD (prior notation *CONSTRAINED_SPR3 still works) Purpose: Define a spotweld with failure. This model includes a plasticity-damage model that reduces the force and moment resultants to zero as the spotweld fails. The location of the spotweld is defined by a single node at the center of two connected sheets. The domain of influence is specified by a radius, which should be approximate- ly equal to the spotweld’s radius. The algorithm does a normal projection from the two sheets to the spotweld node and locates all nodes within the user-defined diameter of influence. The numerical implementation of this model is similar to the SPR2 model (*CONSTRAINED_SPR2). Card 1 1 2 3 4 Variable PID1 PID2 NSID THICK Type I I I F 5 R F 6 7 8 STIFF ALPHA1 MODEL F F F Default none none none none none none none 1.0 Card 2 Variable 1 RN Type F 2 RS F 3 4 5 6 7 8 BETA LCF LCUPF LCUPR DENS INTP F F F F F F Default none none none none none none none none Additional Card for MODEL = 2, 12, or 22. Card 3 1 2 3 4 5 6 7 8 Variable UPFN UPFS ALPHA2 BETA2 UPRN UPRS ALPHA3 BETA3 Type F F F F F F F F Default none none none none none none none none Additional Card for MODEL = 2, 12, or 22. Card 4 1 2 3 4 5 6 7 8 Variable MRN MRS Type F F Default none none VARIABLE DESCRIPTION PID1 PID2 NSID Part ID of first sheet. Part ID of second sheet. Node set ID of spotweld location nodes. THICK Total thickness of both sheets. R Spotweld radius. STIFF Elastic stiffness. Function ID if MODEL > 10. ALPHA1 Scaling factor 𝛼1. Function ID if MODEL > 10. MODEL Material behavior and damage model, see remarks. EQ. 1: SPR3 (default), EQ. 2: SPR4, EQ.11: same as 1 with selected material parameters as functions, EQ.12: same as 2 with selected material parameters as functions, EQ.21: same as 11 with slight modification, see remarks, EQ.22: same as 12 with slight modification, see remarks. RN RS Tensile strength factor. Function ID if MODEL > 10. Shear strength factor. Function ID if MODEL > 10. BETA Exponent for plastic potential 𝛽1. Function ID if MODEL > 10. VARIABLE DESCRIPTION LCF LCUPF LCUPR DENS INTP UPFN UPFS Load curve ID describing force versus plastic displacement: 𝐹0(𝑢̅𝑝𝑙). Load curve ID describing plastic initiation displacement versus 𝑝𝑙(𝜅). Only for MODEL = 1, 11, or 21. mode mixity: 𝑢̅0 Load curve ID describing plastic rupture displacement versus 𝑝𝑙(𝜅). Only for MODEL = 1, 11, or 21. mode mixity: 𝑢̅𝑓 Spotweld density (necessary for time step calculation). Flag for interpolation. EQ.0: linear (default), EQ.1: uniform, EQ.2: inverse distance weighting. 𝑝𝑙,𝑛 . Plastic initiation displacement in normal direction 𝑢̅0,ref 𝑝𝑙,𝑠 . Plastic initiation displacement in shear direction 𝑢̅0,ref ALPHA2 Plastic initiation displacement scaling factor 𝛼2 . BETA2 UPRN UPRS Exponent for plastic initiation displacement 𝛽2. 𝑝𝑙,𝑛 . Plastic rupture displacement in normal direction 𝑢̅𝑓 ,ref 𝑝𝑙,𝑠 . Plastic rupture displacement in shear direction 𝑢̅𝑓 ,ref ALPHA3 Plastic rupture displacement scaling factor 𝛼3 . BETA3 Exponent for plastic rupture displacement 𝛽3. Proportionality factor for dependency RN. Proportionality factor for dependency RS. MRN MRS Remarks: When this feature is used, it is recommended to use the drilling rotation constraint method for the connected components in explicit analysis, i.e. parameter DRCPSID of *CONTROL_SHELL should refer to all shell parts TION_SPOTWELD connections. involved in INTERPOLA- MODEL = 1, 11, or 21 (“SPR3”) This numerical model is similar to the self-piercing rivet model SPR2 but with some differences to make it more suitable for spotwelds. The first difference is symmetric behavior of the spotweld connection, i.e. there is no distinction between a master sheet and a slave sheet. This is done by averaging the normals of both parts and by always distributing the balance moments equally to both sides. The second difference is that there are not only two but three quantities to describe the kinematics, namely the normal relative displacement 𝛿𝑛, the tangential relative displacement 𝛿𝑡, and the relative rotation 𝜔𝑏 - all with respect to the plane-of-maximum opening. I.e. a relative displacement vector is defined as 𝐮 = (𝛿𝑛, 𝛿𝑡, 𝜔𝑏) The third difference is the underlying material model. With the described kinematic quantities, an elastic effective force vector is computed first: 𝐟 ̃ = (𝑓𝑛, 𝑓𝑡, 𝑚𝑏) = STIFF × 𝐮 = STIFF × (𝜹𝒏, 𝜹𝒕, 𝝎𝒃) From that, two resultant forces for normal direction and tangential direction (shear) are computed via Then, a yield function is defined for plastic behavior 𝐹𝑛 = ⟨𝑓𝑛⟩ + 𝛼1𝑚𝑏, 𝐹𝑠 = 𝑓𝑡 𝜙(𝐟 ̃, 𝒖̅pl) = 𝑃(𝐟 ̃) − 𝐹0(𝒖̅pl) ≤ 0 with relative plastic displacement 𝑢̅𝑝𝑙, potential P 𝑃(𝐟 ̃) = [( 𝐹𝑛 𝑅𝑛 ) + ( 𝐹𝑠 𝑅𝑠 𝟏/𝜷 ] ) (cid:448)(cid:1377) (cid:448)(cid:1377)(cid:9)(cid:487)(cid:1135)(cid:981)(cid:10) (cid:487)(cid:1135)(cid:981) (cid:1377) (cid:1377) (cid:12) (cid:487)(cid:1135)(cid:981) (cid:487)(cid:1135)(cid:981) (cid:1401) (cid:487)(cid:1135)(cid:981) Figure 10-12. Force-displacement curve: plasticity and linear damage and isotropic hardening described by load curve LCF : 𝐹0 = 𝐹0(𝒖̅pl) In addition, a linear softening evolution is incorporated, where damage is defined as: pl(𝜅) 𝑑 = 𝑢̅pl − 𝑢̅0 pl(𝜅) 𝑢̅𝑓 , 0 < 𝑑 < 1 with mode mixity 𝜅 = arctan ( 𝐹𝑛 𝐹𝑠 ) , 0 < 𝜅 < 1 Finally, the nominal force is computed as: 𝐟 = (1 − 𝑑)𝐟 ̃ MODEL = 2, 12, or 22 (“SPR4”) In this approach, the relative displacement vector is defined as in model 1 The elastic effective force vector is computed using the elastic stiffness STIFF 𝐟 ̃ = (𝑓𝑛, 𝑓𝑡) = STIFF × 𝐮 = STIFF × (𝜹𝒏, 𝜹𝒕) 𝐮 = (𝛿𝑛, 𝛿𝑡) A yield function is defined for plastic behavior 𝜙(𝐟 ̃, 𝒖̅𝒑𝒍) = 𝑃(𝐟 ̃) − 𝐹0(𝒖̅𝒑𝒍) ≤ 0 with relative plastic displacement 𝑢̅𝑝𝑙, potential P 𝑃(𝐟 ̃) = [( 𝑓𝑛 𝑅̃ 𝑛 𝜷𝟏 ) + ( 𝑓𝑡 𝑅̃ 𝑠 𝟏/𝜷𝟏 ) ] wherein 𝑅̃ 𝑛 and 𝑅̃ 𝑠 represents the load capacity in normal and tangential direction respectively. They are calculated by the values of RN and RS and the influence of relative rotation angle 𝜔𝑏scaled by ALPHA1 𝑅̃ 𝑠 = 𝑅𝑠 𝑅̃ 𝑛 = 𝑅𝑛(1 − 𝛼1 𝜔𝑏) In addition, a linear softening evolution is incorporated, where damage is defined as: 𝑑 = 𝑝𝑙 𝑢̅𝑝𝑙 − 𝑢̅0 𝑝𝑙 𝑢̅𝑓 , 0 < 𝑑 < 1 The calculation of 𝑢̅0 𝑝𝑙 and 𝑢̅𝑓 𝑝𝑙 is done by solving the following equations 𝛽2 𝑝𝑙,𝑛 𝑢̅0 ⎤ ⎡ ⎥ ⎢ 𝑝𝑙,𝑛 (1 − 𝛼2𝜔𝑏)⎦ 𝑢̅0,ref ⎣ ⎧ { ⎨ { ⎩ + 𝑝𝑙,𝑠 ⎜⎜⎜⎛ 𝑢̅0 𝑝𝑙,𝑠 𝑢̅0,𝑟𝑒𝑓 ⎝ ⎟⎟⎟⎞ ⎠ 𝛽2 𝛽2 ⎫ } ⎬ } ⎭ − 1 = 0 𝑝𝑙 𝑝𝑙,𝑛 = sin(𝜑) 𝑢̅0 𝑢̅0 𝑝𝑙 𝑝𝑙,𝑠 = c𝑜𝑠(𝜑)𝑢̅0 𝑢̅0 𝛽3 𝑝𝑙,𝑛 𝑢̅𝑓 ⎤ ⎡ ⎥ ⎢ 𝑝𝑙,𝑛 (1 − 𝛼3𝜔𝑏)⎦ 𝑢̅𝑓 ,𝑟𝑒𝑓 ⎣ ⎧ {{ ⎨ {{ ⎩ + 𝑝𝑙,𝑠 ⎜⎜⎜⎛ 𝑢̅𝑓 𝑝𝑙,𝑠 𝑢̅𝑓 ,𝑟𝑒𝑓 ⎝ 𝛽3 ⎟⎟⎟⎞ ⎠ 𝛽3 ⎫ }} ⎬ }} ⎭ − 1 = 0 considering the load angle 𝜑 𝑝𝑙 𝑝𝑙,𝑛 = sin(𝜑) 𝑢̅𝑓 𝑢̅𝑓 𝑝𝑙 𝑝𝑙,𝑠 = c𝑜𝑠(𝜑)𝑢̅𝑓 𝑢̅𝑓 𝜑 = arctan ( 𝑓𝑛 𝑓𝑠 ) To describe a rate dependent behavior a plastic deformation rate 𝑢̅ ̇𝑝𝑙 is defined by ̇𝑝𝑙 = 𝑢̅ Δ𝑢̅𝑝𝑙 Δ𝑡 wherein Δ𝑢̅𝑝𝑙 is the plastic increment in the current time step and Δ𝑡 is the time step size. If MRN and MRS are defined, the calculation of 𝑅̃ 𝑛 and 𝑅̃ 𝑠 is changed to 𝑅̃ 𝑛(𝑢̅ ̇𝑝𝑙) = (𝑅𝑛 + 𝑚𝑅𝑛𝑢̅ ̇𝑝𝑙)(1 − 𝛼1 𝜔𝑏) ̇𝑝𝑙) = 𝑅𝑠 + 𝑚𝑅𝑠𝑢̅ A detailed description of the SPR4 approach (MODEL = 2) is given in Bier and Sommer [2013], where this model is called “SPR3_IWM”. 𝑅̃ 𝑠(𝑢̅ ̇𝑝𝑙 MODEL > 10 If MODEL is chosen to be greater than 10, then 5 variables have to be defined as function IDs: STIFF, ALPHA1, RN, RS, and BETA. These functions incorporate the following input values: thicknesses of both weld partners (t1, t2) and maximum engineering yield stresses, also called necking points (sm1, sm2). For ALPHA1 = 100 such a function could look like, *DEFINE_FUNCTION 100 func(t1,t2,sm1,sm2)=sm1/sm2 (This function is only a demonstration, it does not make any physical sense). For MODEL = 11 or 12, the master part is the first weld partner represented by t1 and sm1. For MODEL = 21 or 22, the thinner part is the first weld partner. Since material parameters have to be identified from both weld partners during initialization, this feature is only available for a subset of material models at the moment, namely no. 24, 120, 123, and 124. *CONSTRAINED_JOINT_OPTION_{OPTION}_{OPTION}_{OPTION} Available forms include (one is mandatory): *CONSTRAINED_JOINT_SPHERICAL *CONSTRAINED_JOINT_REVOLUTE *CONSTRAINED_JOINT_CYLINDRICAL *CONSTRAINED_JOINT_PLANAR *CONSTRAINED_JOINT_UNIVERSAL *CONSTRAINED_JOINT_TRANSLATIONAL *CONSTRAINED_JOINT_LOCKING *CONSTRAINED_JOINT_TRANSLATIONAL_MOTOR *CONSTRAINED_JOINT_ROTATIONAL_MOTOR *CONSTRAINED_JOINT_GEARS *CONSTRAINED_JOINT_RACK_AND_PINION *CONSTRAINED_JOINT_CONSTANT_VELOCITY *CONSTRAINED_JOINT_PULLEY *CONSTRAINED_JOINT_SCREW If the force output data is to be transformed into a local coordinate use the option: LOCAL to define a joint ID and heading the following option is available: ID and to define failure for penalty-based joints (LMF = 0 in *CONTROL_RIGID) use: FAILURE The ordering of the bracketed options is arbitrary. Purpose: Define a joint between two rigid bodies. *CONSTRAINED Card 1: required for all joint types Card 2: required for joint types: MOTOR, GEARS, RACK_AND_PINION, PULLEY, and SCREW Optional Card: required only if LOCAL is specified in the keyword In the first seven joint types above excepting the Universal joint, the nodal points within the nodal pairs (1, 2), (3, 4), and (5, 6) should coincide in the initial configuration, and the nodal pairs should be as far apart as possible to obtain the best behavior. For the Universal Joint the nodes within the nodal pair (3, 4) do not coincide, but the lines drawn between nodes (1, 3) and (2, 4) must be perpendicular. For the Gear joint the nodes within the nodal pair (1, 2) must not coincide. When the penalty method is used , at each time step, the relative penalty stiffness is multiplied by a function dependent on the step size to give the maximum stiffness that will not destroy the stability of the solution. Instabilities can result in the explicit time integration scheme if the penalty stiffness is too large. If instabilities occur, the recommended way to eliminate these problems is to decrease the time step or reduce the scale factor on the penalties. For cylindrical joints, by setting node 3 to zero, it is possible to use a cylindrical joint to join a node that is not on a rigid body (node 1) to a rigid body (nodes 2 and 4). ID Card. Additional card for ID keyword option. Optional 1 2 3 4 5 6 7 8 Variable JID Type I HEADING A70 The heading is picked up by some of the peripheral LS-DYNA codes to aid in post- processing. VARIABLE DESCRIPTION JID Joint ID. This must be a unique number. HEADING Joint descriptor. It is suggested that unique descriptions be used. Card 1 Variable Type Default 1 N1 I 0 2 N2 I 0 3 N3 I 0 4 N4 I 0 5 N5 I 0 6 N6 I 0 7 8 RPS DAMP F F 1.0 1.0 VARIABLE DESCRIPTION N1 N2 N3 N4 N5 N6 Node 1, in rigid body A. Define for all joint types. Node 2, in rigid body B. Define for all joint types. Node 3, in rigid body A. Define for all joint types except SPHERICAL. Node 4, in rigid body B. Define for all joint types except SPHERICAL. Node 5, in rigid body A. Define for joint types TRANSLATION- AL, LOCKING, ROTATIONAL_MOTOR, CONSTANT_VELOCI- TY, GEARS, RACK_AND_PINION, PULLEY, and SCREW Node 6, in rigid body B. Define for joint types TRANSLATION- AL, LOCKING, ROTATIONAL_MOTOR, CONSTANT_VELOCI- TY, GEARS, RACK_AND_PINION, PULLEY, and SCREW RPS Relative penalty stiffness (default = 1.0): GT.0.0: constant value, LT.0.0: time dependent value given by load curve ID = -RPS (only for SPHERICAL, REVOLUTE, and CYLINDRI- CAL). DAMP Damping scale factor on default damping value. (Revolute and Spherical Joints): EQ.0.0: default is set to 1.0, GT.0.0.AND.LE.0.01: no damping is used. Rotational Properties Card. Additional card for joint types MOTOR, GEARS, RACK_AND_PINION, PULLEY, and SCREW. Card 2 1 2 3 4 5 6 7 8 Variable PARM LCID TYPE R1 H_ANGLE Type F I I F F Default none 0.0 VARIABLE DESCRIPTION PARM Parameter, which a function of joint type: Gears: define 𝑅2/𝑅1 Rack and Pinion: define ℎ Pulley: define 𝑅2/𝑅1 Screw: define 𝑥̇/𝜔 Motors: leave blank Define load curve ID for MOTOR joints. Define integer flag for MOTOR joints as follows: EQ.0: translational/rotational velocity EQ.1: translational/rotational acceleration EQ.2: translational/rotational displacement Radius, 𝑅1, for the gear and pulley joint type. If left undefined, nodal points 5 and 6 are assumed to be on the outer radius. The value of R1 and R2 affect the reaction forces written to output. The forces are calculated from the moments by dividing them by the radii. LCID TYPE R1 H_ANGLE Helix angle in degrees. This is only necessary for the gear joint if the gears do not mesh tangentially, e.g., worm gears, see remarks below for a definition. Local Card. Additional card required for LOCAL keyword option. Card 3 1 2 3 4 5 6 7 8 Variable RAID LST Type Default I 0 I 0 VARIABLE RAID DESCRIPTION Rigid body or accelerometer ID. The force resultants are output in the local system of the rigid body or accelerometer. LST Flag for local system type: EQ.0: rigid body EQ.1: accelerometer Failure Card 1. Additional card for FAILURE keyword option. Card 4 1 2 3 4 5 6 7 8 Variable CID TFAIL COUPL Type Default I 0 F 0 F 0. Failure Card 2. Additional card for FAILURE keyword option. Card 5 1 2 3 4 5 6 7 8 Variable NXX NYY NZZ MXX MYY MZZ Type Default F 0 F 0 F 0 F 0 F 0 F VARIABLE CID DESCRIPTION Coordinate ID for resultants in the failure criteria. If zero, the global coordinate system is used. TFAIL Time for joint failure. If zero, joint never fails. COUPL NXX NYY NZZ MXX MYY MZZ Coupling between the force and moment failure criteria. If COUPL is less than or equal to zero, the failure criteria is identical to the spotwelds. When COUPL is greater than zero, the force and moment results are considered independently. See the remark below. Axial force resultant 𝑁𝑥𝑥𝐹at failure. If zero, failure due to this component is not considered. Force resultant 𝑁𝑦𝑦𝐹 at failure. If zero, failure due to this component is not considered. Force resultant 𝑁𝑧𝑧𝐹 at failure. If zero, failure due to this component is not considered. Torsional moment resultant 𝑀𝑧𝑧𝐹 at failure. If zero, failure due to this component is not considered. Moment resultant 𝑀𝑦𝑦𝐹 at failure. If zero, failure due to this component is not considered. Moment resultant 𝑀𝑧𝑧𝐹 at failure. If zero, failure due to this component is not considered. Node 2 at center The axial direction, e1 The tangential direction, e2 Tangent vector to the teeth e3 Figure 10-13. Helix angle 𝛼 definition, gear #2 viewed from the extension of node 𝑛2 to node 𝑛6. Remarks: The moments for the revolute, cylindrical, planar, translational, and locking joints are calculated at the midpoint of nodes N1 and N3. The moments for the spherical, universal, constant velocity, gear, pulley, and rack and pinion joints are calculated at node N1. When COUPL is less than or equal to zero, the failure criteria is ( 𝑁𝑥𝑥 𝑁𝑥𝑥𝐹 ) + ( 𝑁𝑦𝑦 𝑁𝑦𝑦𝐹 ) + ( 𝑁𝑧𝑧 𝑁𝑧𝑧𝐹 ) + ( 𝑀𝑥𝑥 𝑀𝑥𝑥𝐹 ) + ( 𝑀𝑦𝑦 𝑀𝑦𝑦𝐹 ) + ( 𝑀𝑧𝑧 𝑀𝑧𝑧𝐹 ) − 1 = 0. Otherwise, it consists of both and ( 𝑁𝑥𝑥 𝑁𝑥𝑥𝐹 ) + ( 𝑁𝑦𝑦 𝑁𝑦𝑦𝐹 ) + ( 𝑁𝑧𝑧 𝑁𝑧𝑧𝐹 ) − 1 = 0, ( 𝑀𝑥𝑥 𝑀𝑥𝑥𝐹 ) + ( 𝑀𝑦𝑦 𝑀𝑦𝑦𝐹 ) + ( 𝑀𝑧𝑧 𝑀𝑧𝑧𝐹 ) − 1 = 0. For a gear joint, the relative direction and magnitude of rotation between the two gears is determined by the helix angle. Let 𝐞1 be the unit normal directed from node 2 to 4, which corresponds to the second gear’s rotation axis. See Figure 10-23. Let 𝐞2 be defined as the positively oriented tangent vector to motion of the teeth when spun about the 𝐞1 axis (the gear’s axis). See Figure 10-13. The helix angle 𝛼 characterizes the deviation of the teeth axis from the gear axis. In particular, 𝛼 is defined as the angle between the direction of teeth, called 𝐞3, and the axis of the gear 𝐞1, 𝐞3 = cos𝛼𝐞1 + sin𝛼𝐞2. The gears are assumed to be setup so that the teeth initially fit having matching 𝐞3 directions. A nonzero helix angle is typically used to model worm gears. 1,2 Radial cross section Figure 10-14. Spherical joint. The relative motion of the rigid bodies is constrained so that nodes which are initially coincident remain coincident. In the above figure the socket’s node is not interior to the socket—LS-DYNA does not require that a rigid body’s nodes be interior to the body. Centerline Centerline 3,4 1,2 Figure 10-15. Revolute Joint. Nodes 1 and 2 are coincident; nodes 3 and 4 are coincident. Nodes 1 and 3 belong to rigid body A; nodes 2 and 4 belong to rigid body B. The relative motion of the two rigid bodies is restricted to rotations about the axis formed by the two pairs of coincident nodes. This axis is labeled the “centerline”. Initial Current Centerline 1,2 3,4 Figure 10-16. Cylindrical Joint. This joint is derived from the rotational joint by relaxing the constraints along the centerline. This joint admits relative rotation and translation along the centerline. Initial Current Centerline 1,2 3,4 5,6 Figure 10-17. Translational joint. This is a cylindrical joint with a third pair of off-centerline nodes which restrict rotation. Aside from translation along the centerline, the two rigid bodies are stuck together. Figure 10-18. Planar joint. This joint is derived from the rotational joint by relaxing the constraints normal to the centerline. Relative displacements along the direction of the centerline are excluded. 1,2 Figure 10-19. Universal Joint. Nodes 1 and 2 are initially coincident. The segments formed by nodal pairs (1, 3) and (2, 4) must be orthogonal; they serve as axes about which the two bodies may undergo relative rotation. The universal joint excludes all other relative motion and the axes remain orthogonal at all time. Initial, Final 1,2 5,6 3,43,4 Figure 10-20. Locking Joint. A locking joint couples two rigid bodies in all six degrees-of-freedom. The forces and moments required to form this coupling are written to the jntforc file (*DATABASE_JNTFORC). As stated in the Remarks, forces and moments in jntforc are calculated halfway between N1 and N3. Nodal pairs (1, 2), (3, 4) and (5, 6) must be coincident. The three spatial points corresponding to three nodal pairs must be neither collocated nor collinear. Centerline † Load Curve Time Figure 10-21. Translational motor joint. This joint is usually used in combination with a translational or a cylindrical joint. Node 1 and node 2 belong to the first rigid body and the second rigid body, resp. Furthermore, nodes 1 and 2 must be coincident. Node 3 may belong to either rigid body. The vector from node 2 to node 3 is the direction of relative motion. Node 4 is not used and can be left blank. The value of the load curve may specify any of several kinematic measures; see TYPE. Load curve defines relative rotational motion in radians per unit time. Figure 10-22. Rotational motor joint. This joint can be used in combination with other joints such as the revolute or cylindrical joints. Node 1 at center R1 R2 Node 1 at center Node 2 at center R2 Node 2 at center R1 Figure 10-23. Gear joints. Nodal pairs (1, 3) and (2, 4) define axes that are orthogonal to the gears. Nodal pairs (1, 5) and (2, 6) define vectors in the plane of the gears. The ratio 𝑅2 𝑅1⁄ is specified but need not necessarily correspond to the geometry, if for instance the gear consists of spiral grooves. Note that the gear joint in itself does not maintain the contact point but this requires additional treatment, such as accompanying it with other joints. Node 1 at the center of the pinion Node 2 inside the rack Figure 10-24. Rack and pinion joint. Nodal pair (1, 3) defines the axis of rotation of the first body (the pinion). Nodal pair (1, 5) is a vector in the plane of the pinion and is orthogonal to nodal pair (1, 3). Nodal pair (2, 4) defines the direction of travel for the second body (the rack). Nodal pair (2, 6) is parallel to the axis of the pinion and is thus parallel to nodal pair (1, 3). The value h is specified. The velocity of the rack is ℎ𝜔pinion. 1 2 Figure 10-25. Constant velocity joint. Nodal pairs (1, 3) and (2, 4) define an axes for the constant angular velocity, and nodal pairs (1, 5) are orthogonal vectors. Here nodal points 1 and 2 must be coincident. R2 R1 Node 1 at Center Node 2 at Center Figure 10-26. Pulley joint. Nodal pairs (1, 3) and (2, 4) define axes that are orthogonal to the pulleys. Nodal pairs (1, 5) and (2, 6) define vectors in the plane of the pulleys. The ratio 𝑅2 𝑅1⁄ is specified. Screw Centerline 1,2 5,6 3,4 Figure 10-27. Screw joint. The second body translates in response to the spin of the first body. Nodal pairs (1, 3) and (2, 4) lie along the same axis and nodal pairs (1, 5) and (2, 6) are orthogonal vectors. The helix ratio, 𝑥̇ 𝜔⁄ , is specified. *CONSTRAINED_JOINT $ $$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ $ $$$$ *CONSTRAINED_JOINT_PLANAR $ $$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ $ $ Define a planar joint between two rigid bodies. $ - Nodes 91 and 94 are on rigid body 1. $ - Nodes 21 and 150 are on rigid body 2. $ - Nodes 91 and 21 must be coincident. $ * These nodes define the origin of the joint plane. $ - Nodes 94 and 150 must be coincident. $ * To accomplish this, massless node 150 is artificially created at $ the same coordinates as node 94 and then added to rigid body 2. $ * These nodes define the normal of the joint plane (e.g., the $ vector from node 91 to 94 defines the planes' normal). $ *CONSTRAINED_JOINT_PLANAR $ $...>....1....>....2....>....3....>....4....>....5....>....6....>....7....>....8 $ n1 n2 n3 n4 n5 n6 rps 91 21 94 150 0.000E+00 $ $ *NODE $ nid x y z tc rc 150 0.00 3.00 0.00 0 0 $ *CONSTRAINED_EXTRA_NODES_SET $ pid nsid 2 6 $*SET_NODE_LIST $ sid 6 $ nid1 150 $ $$$ request output for joint force data $ *DATABASE_JNTFORC $ dt/cycl lcdt 0.0001 $ Example 2: $ $$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ $ $$$$ *CONSTRAINED_JOINT_REVOLUTE $ $$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ $ $ Create a revolute joint between two rigid bodies. The rigid bodies must $ share a common edge to define the joint along. This edge, however, must $ not have the nodes merged together. Rigid bodies A and B will rotate $ relative to each other along the axis defined by the common edge. $ $ Nodes 1 and 2 are on rigid body A and coincide with nodes 9 and 10 $ on rigid body B, respectively. (This defines the axis of rotation.) $ $ The relative penalty stiffness on the revolute joint is to be 1.0, $ *CONSTRAINED_JOINT_REVOLUTE $ $...>....1....>....2....>....3....>....4....>....5....>....6....>....7....>....8 $ n1 n2 n3 n4 n5 n6 rps damp 1 9 2 10 1.0 $ $ Note: A joint stiffness is not mandatory for this joint to work. $ However, to see how a joint stiffness can be defined for this $ particular joint, see the corresponding example listed in: $ *CONSTRAINED_JOINT_STIFFNESS_GENERALIZED $ $$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ $ *CONSTRAINED_JOINT_COOR_OPTION_{OPTION}_{OPTION}_{OPTION} Available forms include (one is mandatory): *CONSTRAINED_JOINT_COOR_SPHERICAL *CONSTRAINED_JOINT_COOR_REVOLUTE *CONSTRAINED_JOINT_COOR_CYLINDRICAL *CONSTRAINED_JOINT_COOR_PLANAR *CONSTRAINED_JOINT_COOR_UNIVERSAL *CONSTRAINED_JOINT_COOR_TRANSLATIONAL *CONSTRAINED_JOINT_COOR_LOCKING *CONSTRAINED_JOINT_COOR_TRANSLATIONAL_MOTOR *CONSTRAINED_JOINT_COOR_ROTATIONAL_MOTOR *CONSTRAINED_JOINT_COOR_GEARS *CONSTRAINED_JOINT_COOR_RACK_AND_PINION *CONSTRAINED_JOINT_COOR_CONSTANT_VELOCITY *CONSTRAINED_JOINT_COOR_PULLEY *CONSTRAINED_JOINT_COOR_SCREW If the force output data is to be transformed into a local coordinate use the option: LOCAL to define a joint ID and heading the following option is available: ID and to define failure for penalty-based joints (LMF = 0 in *CONTROL_RIGID) use: FAILURE The ordering of the bracketed options is arbitrary. Purpose: Define a joint between two rigid bodies, see Figure. The connection coordinates are given instead of the nodal point IDs required in the previous section, *CONSTRAINED_JOINT_{OPTION}. Nodes are automatically generated for each coordinate and are constrained to the rigid body. Where coincident nodes are expected in the initial configuration, only one connection coordinate is needed since the connection coordinate for the second node, if given, is ignored. The created nodal ID’s are chosen to exceed the maximum user ID. The coordinates of the joint nodes are specified on Cards 2 - 7. The input which follows Card 7 is identical to that in the previous section. Card Format: Cards 1 - 7: required for all joint types Card 8: required for joint types: MOTOR, GEARS, RACK_AND_PINION, PULLEY, and SCREW Optional Card: required when LOCAL is specified in the keyword In the first seven joint types above excepting the Universal joint, the coordinate points within the nodal pairs (1, 2), (3, 4), and (5, 6) should coincide in the initial configuration, and the nodal pairs should be as far apart as possible to obtain the best behavior. For the Universal Joint the nodes within the coordinate pair (3, 4) do not coincide, but the lines drawn between nodes (1, 3) and (2, 4) must be perpendicular. For the Gear joint the nodes within the coordinate pair (1, 2) must not coincide. When the penalty method is used , at each time step, the relative penalty stiffness is multiplied by a function dependent on the step size to give the maximum stiffness that will not destroy the stability of the solution. LS-DYNA’s explicit time integrator can become unstable when the penalty stiffness is too large. If instabilities occur, the recommended way to eliminate these problems is to decrease the time step or reduce the scale factor on the penalties. For cylindrical joints, by setting node 3 to zero, it is possible to use a cylindrical joint to join a node that is not on a rigid body (node 1) to a rigid body (nodes 2 and 4). ID Card. Additional card for the ID keyword option. Optional 1 2 3 4 5 6 7 8 Variable JID Type I HEADING A70 The heading is picked up by some of the peripheral LS-DYNA codes to aid in post- processing. VARIABLE DESCRIPTION JID Joint ID. This must be a unique number. HEADING Joint descriptor. It is suggested that unique descriptions be used. Card 1 1 2 3 4 5 6 7 8 Variable RBID_A RBID_B RPS DAMP TMASS RMASS Type I I F Card 2 Variable 1 X1 Type F Card 3 Variable 1 X2 Type F Card 4 Variable 1 X3 Type F 2 Y1 F 2 Y2 F 2 Y3 F 3 Z1 F 3 Z2 F 3 Z3 F F 4 F 5 F 6 7 8 4 5 6 7 8 4 5 6 7 Card 5 Variable 1 X4 Type F Card 6 Variable 1 X5 Type F Card 7 Variable 1 X6 Type F 2 Y4 F 2 Y5 F 2 Y6 F 3 Z4 F 3 Z5 F 3 Z6 F 4 5 6 7 8 4 5 6 7 8 4 5 6 7 8 VARIABLE DESCRIPTION RBID_A Part ID of rigid body A. RBID_B Part ID of rigid body B. RPS Relative penalty stiffness (default = 1.0). DAMP Damping scale factor on default damping value. (Revolute and Spherical Joints): EQ.0.0: default is set to 1.0, GT.0.0 and LE.0.01: no damping is used. TMASS RMASS Lumped translational mass. The mass is equally split between the first points defined for rigid bodies A and B. Lumped rotational inertia. The inertia is equally split between the first points defined for rigid bodies A and B. X1, Y1, Z1 Coordinate of point 1, in rigid body A. Define for all joint types. VARIABLE X2, Y2, Z2 DESCRIPTION Coordinate of point 2, in rigid body B. If points 1 and 2 are coincident in the specified joint type, the coordinate for point 1 is used. X3, Y3, Z31 Coordinate of point 3, in rigid body A. Define for all joint types. X4, Y4, Z4 Coordinate of point 4, in rigid body B. If points 3 and 4 are coincident in the specified joint type, the coordinate for point 3 is used. X5, Y5, Z5 Coordinate of point 5, in rigid body A. Define for all joint types. X6, Y6, Z6 Coordinate of point 6, in rigid body B. If points 5 and 6 are coincident in the specified joint type, the coordinate for point 5 is used. Rotational Properties Card. Additional card for joint types MOTOR, GEARS, RACK_AND_PINION, PULLEY, and SCREW. 5 6 7 8 Card 8 1 2 3 Variable PARM LCID TYPE Type F I I 4 R1 F Default none VARIABLE DESCRIPTION PARM Parameter, which a function of joint type: Gears: define 𝑅2/𝑅1 Rack and Pinion: define ℎ Pulley: define 𝑅2/𝑅1 Screw: define 𝑥̇/𝜔 Motors: leave blank LCID Define load curve ID for MOTOR joints. VARIABLE DESCRIPTION TYPE Define integer flag for MOTOR joints as follows: EQ.0: translational/rotational velocity EQ.1: translational/rotational acceleration EQ.2: translational/rotational displacement R1 Radius, 𝑅1, for the gear and pulley joint type. If left undefined, nodal points 5 and 6 are assumed to be on the outer radius. R1 is the moment arm that goes into calculating the joint reaction forces. The ratio R2/R1 gives the transmitted moments, but not the forces. The force is moment divided by distance R1. Local Card. Additional card for LOCAL keyword option. Card 9 1 2 3 4 5 6 7 8 Variable RAID LST Type Default I 0 I 0 VARIABLE RAID DESCRIPTION Rigid body or accelerometer ID. The force resultants are output in the local system of the rigid body or accelerometer. LST Flag for local system type: EQ.0: rigid body EQ.1: accelerometer Failure Card 1. Additional card for the FAILURE keyword option. Card 10 1 2 3 4 5 6 7 8 Variable CID TFAIL COUPL Type Default I 0 F 0 F 0. Failure Card 2. Additional card for the FAILURE keyword option. Card 11 1 2 3 4 5 6 7 8 Variable NXX NYY NZZ MXX MYY MZZ Type Default F 0 F 0 F 0 F 0 F 0 F 0 VARIABLE CID DESCRIPTION Coordinate ID for resultants in the failure criteria. If zero, the global coordinate system is used. TFAIL Time for joint failure. If zero, joint never fails. COUPL NXX NYY NZZ Coupling between the force and moment failure criteria. If COU- PL is less than or equal to zero, the failure criteria is identical to the spotwelds. When COUPL is greater than zero, the force and moment results are considered independently. See the remarks in *CONSTRAINED_JOINT_{OPTION}. Axial force resultant 𝑁𝑥𝑥𝐹at failure. If zero, failure due to this component is not considered. Force resultant 𝑁𝑌𝑌𝐹 at failure. If zero, failure due to this component is not considered. Force resultant 𝑁𝑧𝑧𝐹 at failure. If zero, failure due to this component is not considered. VARIABLE DESCRIPTION MXX MYY MZZ Torsional moment resultant 𝑀𝑋𝑋𝐹 at failure. If zero, failure due to this component is not considered. Moment resultant 𝑀𝑌𝑌𝐹 at failure. If zero, failure due to this component is not considered. Moment resultant 𝑀𝑍𝑍𝐹 at failure. If zero, failure due to this component is not considered. *CONSTRAINED_JOINT_STIFFNESS_OPTION_{OPTION} Available options include: FLEXION-TORSION GENERALIZED TRANSLATIONAL If desired a description of the joint stiffness can be provided with the option: TITLE which is written into the d3hsp and jntforc files. Purpose: Define optional rotational and translational joint stiffness for joints defined by *CONSTRAINED_JOINT_OPTION. These definitions apply to all joints even though degrees of freedom that are considered in the joint stiffness capability may be constrained out in some joint types. The energy that is dissipated with the joint stiffness option is written for each joint in joint force file with the default name, jntforc. In the global energy balance this energy is included with the energy of the discrete elements, i.e., the springs and dampers. Card Format: The optional TITLE card and card 1 are common to all joint stiffness types. Cards 2 to 4 are unique for each stiffness type. Title Card. Additional card for the TITLE keyword option. Optional 1 2 3 4 5 6 7 8 Variable Type TITLE A80 Card 1 1 2 3 4 5 6 7 8 Variable JSID PIDA PIDB CIDA CIDB JID Type I I I I I I Default none none none none CIDA none VARIABLE DESCRIPTION TITLE Description of joint stiffness for output files jntforc and d3hsp. JSID PIDA PIDB CIDA CIDB Joint stiffness ID Part ID for rigid body A, see *PART. Part ID for rigid body B, see *PART. Coordinate ID for rigid body A, see *DEFINE_COORDINATE_- OPTION. For the translational stiffness the local coordinate system must be defined by nodal points, *DEFINE_COORDI- NATE_NODES, since the first nodal point in each coordinate system is used to track the motion. Coordinate ID for rigid body B. If zero, the coordinate ID for rigid body A is used, see *DEFINE_COORDINATE_OPTION. For the translational stiffness the local coordinate system must be defined by nodal points, *DEFINE_COORDINATE_NODES, since the first nodal point in each coordinate system is used to track the motion. JID Joint ID for the joint reaction forces. If zero, tables can’t be used in place of load curves for defining the frictional moments. Card 2 for FLEXION-TORSION option. Card 2 1 2 3 4 5 6 7 8 Variable LCIDAL LCIDG LCIDBT DLCIDAL DLCIDG DLCIDBT Type I I I I I I Default none 1.0 none none 1.0 none Card 3 for FLEXION-TORSION option. Card 3 1 2 3 4 5 6 7 8 Variable ESAL FMAL ESBT FMBT Type F F F F Default 0.0 0.0 0.0 0.0 Card 4 for FLEXION-TORSION option. Card 4 1 2 3 4 5 6 7 8 Variable SAAL NSABT PSABT Type F F F Default not used not used not used Figure 10-28. The angles 𝛼, 𝛽, 𝛾 align rigid body one with rigid body two for the FLEXION-TORSION option. VARIABLE LCIDAL LCIDG LCIDBT DLCIDAL DLCIDG DESCRIPTION Load curve ID for 𝛼-moment versus rotation in radians. See Figure 10-28 where it should be noted that 0 ≤ 𝛼 ≤ 𝜋. If zero, the applied moment is set to zero. See *DEFINE_CURVE. Load curve ID for 𝛾 versus a scale factor which scales the bending moment due to the 𝛼 rotation. This load curve should be defined in the interval −𝜋 ≤ 𝛾 ≤ 𝜋. If zero the scale factor defaults to 1.0. See *DEFINE_CURVE. Load curve ID for 𝛽-torsion moment versus twist in radians. If zero the applied twist is set to zero. See *DEFINE_CURVE. Load curve ID for 𝛼-damping moment versus rate of rotation in radians per unit time. If zero, damping is not considered. See *DEFINE_CURVE. Load curve ID for 𝛾-damping scale factor versus rate of rotation in radians per unit time. This scale factor scales the 𝛼-damping moment. If zero, the scale factor defaults to one. See *DEFINE_- CURVE. DLCIDBT Load curve ID for 𝛽-damping torque versus rate of twist. If zero damping is not considered. See *DEFINE_CURVE. z1 z2 y2 x1 y1 x2 Figure 10-29. Flexion-torsion joint angles. If the initial positions of the local coordinate axes of the two rigid bodies connected by the joint do not coincide, the angles, 𝛼 and 𝛾, are initialized and torques will develop instantaneously based on the defined load curves. The angle 𝛽 is also initialized but no torque will develop about the local axis on which 𝛽 is measured. Rather, 𝛽 will be measured relative to the computed offset. VARIABLE ESAL FMAL DESCRIPTION Elastic stiffness per unit radian for friction and stop angles for 𝛼 rotation. If zero, friction and stop angles are inactive for 𝛼 rotation. See Figure 10-31. Frictional moment limiting value for 𝛼 rotation. If zero, friction is inactive for 𝛼 rotation. This option may also be thought of as an elastic-plastic spring. If a negative value is input then the absolute value is taken as the load curve or table ID defining the yield moment versus 𝛼 rotation. A table permits the moment to also be a function of the joint reaction force and requires the specification of JID on Card 1. See Figure 10-31. VARIABLE DESCRIPTION ESBT FMBT Elastic stiffness per unit radian for friction and stop angles for 𝛽 twist. If zero, friction and stop angles are inactive for 𝛽 twist. Frictional moment limiting value for 𝛽 twist. If zero, friction is inactive for 𝛽 twist. This option may also be thought of as an elastic-plastic spring. If a negative value is input then the absolute value is taken as the load curve or table ID defining the yield moment versus 𝛽 rotation. A table permits the moment to also be a function of the joint reaction force and requires the specification of JID on Card 1. SAAL Stop angle in degrees for 𝛼 rotation where 0 ≤ 𝛼 ≤ 𝜋. Ignored if zero. See Figure 10-31. NSABT Stop angle in degrees for negative 𝛽 rotation. Ignored if zero. PSABT Stop angle in degrees for positive 𝛽 rotation. Ignored if zero. Remarks: This option simulates a flexion-torsion behavior of a joint in a slightly different fashion than with the generalized joint option. After the stop angles are reached the torques increase linearly to resist further angular motion using the stiffness values on Card 3. If the stiffness value is too low or zero, the stop will be violated. The moment resultants generated from the moment versus rotation curve, damping moment versus rate-of-rotation curve, and friction are evaluated independently and are added together. Card 2 for GENERALIZED stiffness option. Card 2 1 2 3 4 5 6 7 8 Variable LCIDPH LCIDT LCIDPS DLCIDPH DLCIDT DLCIDPS Type I I I I I I Default none none none none none none Figure 10-30. Definition of angles for the GENERALIZED joint stiffness. Card 3 for GENERALIZED stiffness option. Card 3 1 2 3 4 5 6 7 8 Variable ESPH FMPH EST FMT ESPS FMPS Type F F F F F F Default 0.0 0.0 0.0 0.0 0.0 0.0 Card 4 for GENERALIZED stiffness option. Card 4 1 2 3 4 5 6 7 8 Variable NSAPH PSAPH NSAT PSAT NSAPS PSAPS Type Default F 0 F 0 F 0 F 0 F 0 F Case I: Elastic Perfectly Plastic Yield Curve Case II: Load Curve Used for Yield Curve friction value elastic stiffness load curve Displacement negative stop displacement Displacement positive stop displacement negative stop negative stop displacement displacement positive stop positive stop displacement displacement Yield curve beyond stop angle Yield curve Example loading/unloading path load curve reflection Figure 10-31. Friction model. The friction model is motivated by plasticity and it is implemented for both rotational and translational joints. In the context of a rotational joint, the y-axis is to be interpreted as moment (rotational force) and the x-axis is to be interpreted as rotation. Case I (left) is activated by a positive friction value. Case II (right) is activated by a negative integer friction value, the absolute value of which specifies a load curve. See the friction, elastic, and stop angle/displacement parameters from the input cards (FM[var], ES[var], NSA[var], PSA[var]). VARIABLE LCIDPH LCIDT LCIDPS DLCIDPH DLCIDT DESCRIPTION Load curve ID for 𝜙-moment versus rotation in radians. See Figure 10-30. If zero, the applied moment is set to 0.0. See *DE- FINE_CURVE. Load curve ID for 𝜃-moment versus rotation in radians. If zero, the applied moment is set to 0.0. See *DEFINE_CURVE. Load curve ID for 𝜓-moment versus rotation in radians. If zero, the applied moment is set to 0.0. See *DEFINE_CURVE. Load curve ID for 𝜙-damping moment versus rate of rotation in radians per unit time. If zero, damping is not considered. See *DEFINE_CURVE. Load curve ID for 𝜃-damping moment versus rate of rotation in radians per unit time. If zero, damping is not considered. See *DEFINE_CURVE. VARIABLE DLCIDPS ESPH FMPH EST FMT ESPS FMPS DESCRIPTION Load curve ID for 𝜓-damping torque versus rate of rotation in radians per unit time. If zero, damping is not considered. See *DEFINE_CURVE. Elastic stiffness per unit radian for friction and stop angles for 𝜙 rotation. If zero, friction and stop angles are inactive for 𝜙 rotation. Frictional moment limiting value for 𝜙 rotation. If zero, friction is inactive for 𝜙 rotation. This option may also be thought of as an elastic-plastic spring. If a negative value is input then the absolute value is taken as the load curve or table ID defining the yield moment versus 𝜙 rotation. A table permits the moment to also be a function of the joint reaction force and requires the specification of JID on card 1. See Figure 10-31. Elastic stiffness per unit radian for friction and stop angles for 𝜃 rotation. If zero, friction and stop angles are inactive for 𝜃 rotation. See Figure 10-31. Frictional moment limiting value for 𝜃 rotation. If zero, friction is inactive for 𝜃 rotation. This option may also be thought of as an elastic-plastic spring. If a negative value is input then the absolute value is taken as the load curve or table ID defining the yield moment versus 𝜃 rotation. A table permits the moment to also be a function of the joint reaction force and requires the specification of JID on card 1. Elastic stiffness per unit radian for friction and stop angles for 𝜓 rotation. If zero, friction and stop angles are inactive for 𝜓 rotation. Frictional moment limiting value for 𝜓 rotation. If zero, friction is inactive for 𝜓 rotation. This option may also be thought of as an elastic-plastic spring. If a negative value is input then the absolute value is taken as the load curve or table ID defining the yield moment versus 𝜓 rotation. A table permits the moment to also be a function of the joint reaction force and requires the specification of JID on card 1. NSAPH Stop angle in degrees for negative 𝜙 rotation. Ignored if zero. See Figure 10-31. PSAPH Stop angle in degrees for positive 𝜙 rotation. Ignored if zero. VARIABLE DESCRIPTION NSAT PSAT Stop angle in degrees for negative 𝜃 rotation. Ignored if zero. Stop angle in degrees for positive 𝜃 rotation. Ignored if zero. NSAPS Stop angle in degrees for negative 𝜓 rotation. Ignored if zero. PSAPS Stop angle in degrees for positive 𝜓 rotation. Ignored if zero. Remarks: After the stop angles are reached the torques increase linearly to resist further angular motion using the stiffness values on Card 3. Reasonable stiffness values have to be chosen. If the stiffness values are too low or zero, the stop will be violated. If the initial local coordinate axes do not coincide, the angles, 𝜙, 𝜃, and 𝜓, will be initialized and torques will develop instantaneously based on the defined moment vs. rotation curves. There are two methods available to calculate the rotation angles between the coordinate systems. For more information, see the JNTF parameter on *CONTROL_RIGID. Card 2 for TRANSLATIONAL stiffness option. Card 2 1 2 3 4 5 6 7 8 Variable LCIDX LCIDY LCIDZ DLCIDX DLCIDY DLCIDZ Type I I I I I I Default none none none none none none Card 3 TRANSLATIONAL stiffness option. Card 3 1 2 3 4 5 6 7 8 Variable ESX FFX ESY FFY ESZ FFZ Type F F F F F F Default 0.0 0.0 0.0 0.0 0.0 0.0 Card 4 for TRANSLATIONAL stiffness option. Card 4 1 2 3 4 5 6 7 8 Variable NSDX PSDX NSDY PSDY NSDZ PSDZ Type Default F 0 F 0 F 0 F 0 F 0 F 0 VARIABLE LCIDX LCIDY LCIDZ DLCIDX DESCRIPTION Load curve ID for x-force versus x-distance between the origins of CIDA and CIDB based on the x-direction of CIDB. If zero, the applied force is set to 0.0. See *DEFINE_CURVE. Load curve ID for y-force versus y-distance between the origins of CIDA and CIDB based on the y-direction of CIDB. If zero, the applied force is set to 0.0. See *DEFINE_CURVE. Load curve ID for z-force versus z-distance between the origins of CIDA and CIDB based on the z-direction of CIDB. If zero, the applied force is set to 0.0. See *DEFINE_CURVE. Load curve ID for x-damping force versus rate of x-translational displacement per unit time between the origins of CIDA and CIDB based on the x-direction of CIDB. If zero, damping is not considered. See *DEFINE_CURVE. VARIABLE DLCIDY DLCIDZ ESX FFX ESY FFY ESZ FMZ DESCRIPTION Load curve ID for y-damping force versus rate of y-translational displacement per unit time between the origins of CIDA and CIDB based on the y-direction of CIDB. If zero, damping is not considered. See *DEFINE_CURVE. Load curve ID for z-damping force versus rate of z-translational displacement per unit time between the origins of CIDA and CIDB based on the z-direction of CIDB. If zero, damping is not considered. See *DEFINE_CURVE. Elastic stiffness for friction and stop displacement for x- translation. If zero, friction and stop angles are inactive for x- translation. See Figure 10-31. Frictional force limiting value for x-translation. If zero, friction is inactive for x-translation. This option may also be thought of as an elastic-plastic spring. If a negative value is input then the absolute value is taken as the load curve ID defining the yield force versus x-translation. See Figure 10-31. Elastic stiffness for friction and stop displacement for y- translation. If zero, friction and stop angles are inactive for y- translation. Frictional force limiting value for y-translation. If zero, friction is inactive for y-translation. This option may also be thought of as an elastic-plastic spring. If a negative value is input then the absolute value is taken as the load curve ID defining the yield force versus y-translation. Elastic stiffness for friction and stop displacement for z- translation. If zero, friction and stop angles are inactive for z- translation. Frictional force limiting value for z-translation. If zero, friction is inactive for z-translation. This option may also be thought of as an elastic-plastic spring. If a negative value is input then the absolute value is taken as the load curve ID defining the yield force versus z-translation. NSDX Stop displacement for negative x-translation. Ignored if zero. See Figure 10-31. PSDX Stop displacement for positive x-translation. Ignored if zero. VARIABLE DESCRIPTION Stop displacement for negative y-translation. Ignored if zero. Stop displacement for positive y-translation. Ignored if zero. Stop displacement for negative z-translation. Ignored if zero. Stop displacement for positive z-translation. Ignored if zero. NSDY PSDY NSDZ PSDZ Remarks: After the stop displacements are reached the force increases linearly to resist further translational motion using the stiffness values on Card 3. Reasonable stiffness values must be chosen. If the stiffness values are too low or zero, the stop will be violated. Example: $ $$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ $ $$$$ *CONSTRAINED_JOINT_STIFFNESS_GENERALIZED $ $$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ $ $ Define a joint stiffness for the revolute joint described in $ *CONSTRAINED_JOINT_REVOLUTE $ $ Attributes of the joint stiffness: $ - Used for defining a stop angle of 30 degrees rotation $ (i.e., the joint allows a positive rotation of 30 degrees and $ then imparts an elastic stiffness to prevent further rotation) $ - Define between rigid body A (part 1) and rigid body B (part 2) $ - Define a local coordinate system such that local x corresponds $ to the joint’s axis of revolution and the angle phi is the angle $ of rotation about that axis. $ - The elastic stiffness per unit radian for the stop angle is 100. $ - Variables left blank are not used during the simulation. $ *CONSTRAINED_JOINT_STIFFNESS_GENERALIZED $ $...>....1....>....2....>....3....>....4....>....5....>....6....>....7....>....8 $ jsid pida pidb cida cidb 1 1 2 5 5 $ $ lcidph lcidt lcidps dlcidph dlcidt dlcidps $ $ esph fmps est fmt esps fmps 100.0 $ $ nsaph psaph nsat psat nsaps psaps 30.0 $ $ *DEFINE_COORDINATE_NODES $ cid n1 n2 n3 5 1 2 3 $ $$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ $ *CONSTRAINED_JOINT_USER_FORCE Purpose: Define input data for a user subroutine to generate force resultants as a function of time and joint motion. Card 1 1 2 3 4 5 6 7 8 Variable FID JID NHISV Type I I Default none none I 0 User Subroutine Constants Cards. Define up to 48 optional user constants (6 cards total) for the user subroutine. This input is terminated after 48 constants are defined or when the next “*” keyword card is encountered. Card 2 1 2 3 4 5 6 7 8 Variable CONST1 CONST2 CONST3 CONST4 CONST5 CONST6 CONST7 CONST8 Type F F F F F I I F Default 0.0 0.0 0.0 0.0 0.0 0.0 0.0 0.0 VARIABLE DESCRIPTION FID JID NHISV Joint user force ID. Joint ID for which this user force input applies. Number of history variables required for this definition. An array NHISV long is allocated and passed into the user subroutine. This array is updated in the user subroutine. CONSTn A constant which is passed into the user subroutine. *CONSTRAINED_LAGRANGE_IN_SOLID_{OPTION1}_{OPTION2} Purpose: This command provides the coupling mechanism for modeling Fluid- Structure Interaction (FSI). The structure can be constructed from Lagrangian shell and/or solid entities. The multi-material fluids are modeled by ALE formulation. Available options for OPTION1 include: <BLANK> EDGE This option may be used to allow the coupling between the edge of a shell part or part set and one or more ALE multi-material groups (AMMG). It accounts for the shell thickness in the coupling calculation. The edge thickness is the same as the shell thickness. This option only works when the Lagrangian slave set is defined as a part or a part set ID. It will not work for a slave segment set. One application of this option is a simulation of a Lagrangian blade (a shell part) cutting through some ALE material. Available options for OPTION2 include: <BLANK> TITLE To define a coupling (card) ID number and title for each coupling card. If a title is not defined LS-DYNA will automatically create an internal title for this coupling definition. The ID number can be used to delete coupling action in a restart input deck via the *DELETE_FSI card. Title Card. Additional card for the TITLE keyword option. Optional 1 2 3 4 5 6 7 8 Variable COUPID Type I TITLE A70 Card 1 1 2 3 4 5 6 7 8 Variable SLAVE MASTER SSTYP MSTYP NQUAD CTYPE DIREC MCOUP Type I I Default none none Card 2 1 2 I 0 3 I 0 4 I 0 5 I 2 6 I 1 7 I 0 8 Variable START END PFAC FRIC FRCMIN NORM NORMTYP DAMP Type Default Card 3 Variable Type F 0 1 K F F F F F 1.0E10 0.1 0.0 0.5 2 3 4 5 I 0 6 I 0 7 F 0.0 8 HMIN HMAX ILEAK PLEAK LCIDPOR NVENT IBLOCK Default 0.0 none none F F I 0 F 0.1 I 0 I 0 I 0 Card 4a. This card is required for CTYPE 11 & 12 but is otherwise optional. Card 4a 1 2 3 4 5 6 7 8 Variable IBOXID IPENCHK INTFORC IALESOF LAGMUL PFACMM THKF Type Default I 0 I 0 I 0 I 0 F 0.0 I 0 F 0.0 Porous Coupling Card 4b. This card applies only to CTYPE 11 & 12. If 4b is defined, 4a must be defined before 4b. Card 4b Variable 1 A1 Type F 2 B1 F 3 A2 F 4 B2 F 5 A3 F 6 B3 F Default 0.0 0.0 0.0 0.0 0.0 0.0 7 8 POREINI F 0.0 Venting Geometry Card(s) 4c. These card(s) set venting geometry. It is repeated NVENT times (one card for defining each vent hole). It is defined only if NVENT > 0 in card 3. The last NVENT cards for *CONSTRAINED_LAGRANGE_IN_SOLID are taken to be Card(s) 4c, therefore, Cards 4a and 4b are not mandatory when Card(s) 4c are defined. Card 4c 1 2 3 4 5 6 7 8 Variable VENTSID VENTYP VTCOEF POPPRES COEFLC Type Default I 0 I 0 I 0 F 0.0 I 0 VARIABLE COUPID DESCRIPTION Coupling (card) ID number. This ID can be used in a restart input deck to delete or reactivate this coupling action via the *DELETE_FSI card. If not defined, LSDYNA will assign an internal coupling ID based on the order of appearance in the input deck. TITLE A description of this coupling definition (A70). SLAVE Slave set ID defining a part, part set or segment set ID of the Lagrangian or slave structure . See Remark 1. MASTER Master set ID defining a part or part set ID of the ALE or master solid elements . VARIABLE DESCRIPTION SSTYP Slave set type of “SLAVE” : EQ.0: part set ID (PSID). EQ.1: part ID (PID). EQ.2: segment set ID (SGSID). MSTYP Master set type of “MASTER” : EQ.0: part set ID (PSID). EQ.1: part ID (PID). NQUAD Number of coupling points distributed over each coupled Lagrangian surface segment. EQ.0: NQUAD will be set by default to 2, GT.0: An NQUAD × NQUAD coupling points distribution over each Lagrangian segment is defined, LT.0: NQUAD is reset to a positive value. Coupling at nodes is obsolete. CTYPE Fluid-Structure coupling method. The constraint methods (1, 2, and 3) are not supported in MPP. EQ.1: constrained acceleration. EQ.2: constrained acceleration and velocity (default, see Remark 3). EQ.3: constrained acceleration and velocity, normal direction only. EQ.4: penalty coupling for shell (with or without erosion) and solid elements (without erosion). NOTE: For RIGID slave PARTS a penalty cou- pling method (CTYPE=4) must be used, see parameter CTYPE below. EQ.5: penalty coupling allowing erosion in the Lagrangian entities (solid elements and thick shells). EQ.6: penalty coupling designed for airbag modeling which automatically controls the DIREC parameter internally. It is equivalent to setting {CTYPE = 4; DIREC = 1} for unfolded region; and {CTYPE = 4; DIREC = 2}; in fold- VARIABLE DESCRIPTION ed region. For both cases: {ILEAK = 2; FRCMIN = 0.3}. EQ.11: coupling designed to couple Lagrangian porous shell to ALE material. When this option is used, THKF, the 7th column parameter of optional card 4a and the first 2 parameters of optional card 4b must be defined. See *LOAD_BODY_POROUS and remark 13 below. EQ.12: coupling designed to couple Lagrangian porous solid to ALE material. When this option is used, Ai & Bi pa- rameters of optional card 4b must be defined (card 4a must be defined but can be blank). See *LOAD_- BODY_POROUS and Remark 14 below DIREC For CTYPE=4, 5, or 6 Coupling direction: EQ.1: normal direction, compression and tension (default) EQ.2: normal direction, compression only EQ.3: all directions For CTYPE=12 Flag to activate an element coordinate system: EQ.0: The forces are applied in the global directions. EQ.1: The forces are applied in a local system attached to the Lagrangian solid. is consistent with The system AOPT = 1 in *LOAD_BODY_POROUS. . MCOUP For CTYPE = 4, 5, 6, 11, or 12 Multi-material option: EQ.0: couple with all multi-material groups, EQ.1: couple with material with highest density. LT.0: MCOUP must be an integer. -MCOUP refers to a set ID of an ALE multi-material group. See *SET_MULTI-MA- TERIAL_GROUP. START Start time for coupling. END End time for coupling. If less than zero, coupling will be turned off during dynamic relaxation. After dynamic relaxation phase is finished, the absolute value will be taken as end time. VARIABLE PFAC DESCRIPTION For CTYPE = 4,5 or 6 Penalty factor. PFAC is a scale factor for scaling the estimated stiffness of the interacting (coupling) system. It is used to compute the coupling forces to be distributed on the slave and master parts GT.0: Fraction of estimated critical stiffness. LT.0: PFAC must be an integer, and -PFAC is a load curve ID. The curve defines the coupling pressure on the y-axis as a function of the penetration along the x-axis. For CTYPE = 11 or 12 Time step factor FRIC Coefficient of friction (used with DIREC = 1 and 2 only). FRCMIN Minimum volume fraction of a coupled ALE multi-material group (AMMG) or fluid in a multi-material ALE element to activate coupling. Default value is 0.5. Reducing FRCMIN (typically, between 0.1 and 0.3) would turn on coupling earlier to prevent leakage in high velocity impact cases. NORM A Lagrangian segment will couple to fluid on only one side of the segment. NORM determines which side. See Remark 6. EQ.0: Couple to fluid (AMMG) on head-side of Lagrangian segment normal vector. EQ.1: Couple to fluid (AMMG) on tail-side of Lagrangian segment normal vector. NORMTYP Penalty coupling spring (or force) direction (DIREC = 1, or 2): EQ.0: normal vectors are interpolated from nodal normals. (default). EQ.1: normal vectors are interpolated from segment normals. This is sometimes a little more robust for sharp Lagran- gian corners, and folds. DAMP Damping factor for penalty coupling. This is a coupling-damping scaling factor. Typically it may be between 0 and 1 . VARIABLE DESCRIPTION K HMIN Thermal conductivity of a virtual fluid between the slave surface and the master material . The absolute value is minimum air gap in heat transfer, ℎmin . LT.0: turn on constraint based thermal nodal coupling between LAG structure and ALE fluids. GE.0: minimum air gap. If zero, default to 1.0e-6. HMAX Maximum air gap in heat transfer, ℎmax. There is no heat transfer above this value . ILEAK Coupling leakage control flag (Remark 9): EQ.0: none (default), EQ.1: weak, leakage control is turned off if penetrating volume fraction > FRCMIN + 0.2 EQ.2: strong, with improved energy consideration. Leakage control is turned off if penetrating volume fraction > FRCMIN + 0.4 PLEAK Leakage control penalty factor, 0 < PLEAK < 0.2 is recommended. This factor influences the additional coupling force magnitude to prevent leakage. It is conceptually similar to PFAC. Almost always, the default value (0.1) is adequate. LCIDPOR If this is a positive integer: A load curve ID (LCID) defining porous flow through coupling segment: Abscissa = 𝑥 = (𝑃up − 𝑃down) Ordinate = 𝑦 = relative porous fluid velocity Where Pup and Pdown are, respectively, the upstream and downstream pressures across of the porous coupling segment. The relative porous velocity is the ALE fluid velocity relative to the moving Lagrangian segment. This experimental data curve must be provided by the user. If LCIDPOR is a negative integer: The porous flow is controlled by the parameters FLC, FAC, ELA under *MAT_FABRIC card. VARIABLE DESCRIPTION CAUTION: The pressure under the FAC load curve is “absolute upstream pressure” . Abscissa = 𝑥 = absolute upstream pressure Ordinate = 𝑦 = relative porous fluid velocity For CTYPE = 11 or CTYPE = 12 and POREINI = 0.0: LT.0: The load curve |LCIDPOR| is a factor versus time of the porous force computed by the Ergun equation . GT.0: The load curve LCIDPOR is a porous force versus velocity, which replaces the force computed by the Ergun equation . For CTYPE = 11 or CTYPE = 12 and POREINI > 0.0: NE.0: The load curve |LCIDPOR| is a factor versus time of the porous force computed by the Ergun equation . The number of vent surface areas to be defined. Each venting flow surface is represented by one or more Lagrangian segments (or surfaces). For airbag applications, this may be referred to as “isentropic” venting where the isentropic flow equation is used to compute the mass flow rate based on the ratio of the upstream and downstream pressures 𝑃up/𝑃down. For each of the NVENT vent surfaces, an additional card of format 4c defining the geometrical and flow properties for each vent surface will be read in. The vented mass will simply be deleted from the system and cannot be visualized as in the case of physical venting . NVENT VARIABLE IBLOCK DESCRIPTION Flag to control the venting (or porous) flow blockage due to Lagrangian contact during ALE computation. EQ.0: Off EQ.1: On The venting definition is defined in this command. However, the venting flow may be defined via either the LCIDPOR parameter in this command or via the *MAT_FABRIC parameters (FLC, FAC, ELA). However, note that FVOPT (blocking) parameter under *MAT_FABRIC applies only to CV computation. IBOXID A box ID defining a box region in space in which ALE coupling is activated. GT.0: At time = 0.0, the Lagrangian segments inside this box are remembered. In subsequent coupling computation steps, there is no need to search for the Lagrangian seg- ments again. LT.0: At each FSI bucketsort, the Lagrangian segments inside this box are marked as active coupling segments. This makes the coupling operate more efficiently when struc- ture mesh is approaching ALE domain, i.e. hydroplan- ing, bird strike, etc. IPENCHK Only for CTYPE = 4 Initial penetration check flag : EQ.0: Do not check for initial penetration. EQ.1: Check and save initial ALE material penetration across a Lagrangian surface (d0), but do not activate coupling at t = 0. In subsequent steps (t > 0) the actual penetration is computed as follows: Actual Penetration ⏟⏟⏟⏟⏟⏟⏟⏟⏟ 𝑑𝑎 = Total Penetration ⏟⏟⏟⏟⏟⏟⏟⏟⏟ 𝑑𝑇 − Initial Penetration ⏟⏟⏟⏟⏟⏟⏟⏟⏟ 𝑑0 INTFORC A flag to turn on or off the output of ALE coupling pressure and forces on the slave Lagrangian segments (or surfaces). EQ.0: Off EQ.1: On Note that the coupling pressures and forces are computed based VARIABLE DESCRIPTION on the coupling stiffness reponse to the ALE fluid penetration. When INFORC = 1 and a *DATABASE_BINARY_FSIFOR (DBF) card is defined, LS-DYNA writes out the segment coupling pressure and forces to the binary interface force file for contour plotting. This interface force file must be given a name on the execution line, for example: ls-dyna i=inputfilename.k … h=interfaceforcefilename The time interval between output is defined by “dt” in the DBF card. To plot the binary data in this file: ls-prepost interfaceforcefilename IALESOF An integer flag to turn ON/OFF a supplemental Lagrange multiplier FSI constraint which provides a coupling force in addition to the basic penalty coupling contribution. This is a hybrid coupling method. EQ.0: OFF (default). EQ.1: Turn ON the hybrid Lagrange-multiplier method. LAGMUL multiplier factor is read. LAGMUL A Lagrange multiplier factor with a range between 0.0 and 0.05 may be defined. A typical value may be 0.01. This should never be greater than 0.1. EQ.0: OFF (default). GT.0: Turn ON the Lagrange-multiplier method and use LAGMUL as a coefficient for scaling the penalty factor. PFACMM Mass-based penalty stiffness factor computational options. This works in conjunction with PFAC = constant (not a load curve). The coupling penalty stiffness (CPS) is computed based on an estimated effective coupling mass. EQ.0: CPS ∝ PFAC × min (𝑚slave, 𝑚master) , default. EQ.1: CPS ∝ PFAC × max (𝑚slave, 𝑚master) . EQ.2: CPS ∝ PFAC × √𝑚slave𝑚master , geometric-mean of the masses. EQ.3: CPS ∝ PFAC × 𝐾Lagrangian where K is the bulk modulus of the slave or Lagrangian part VARIABLE THKF DESCRIPTION For all CTYPE choices except 11: A flag to account for the coupling thickness of the Lagrangian shell (slave) part. LT.0: Use positive value of |THKF| for coupling segment thickness. EQ.0: Do not consider coupling segment thickness. GT.0: Coupling segment thickness scale factor. For CTYPE = 11: This thickness is required for volume calculation. GT.0: (Fabric) Thickness scale factor. The base shell thickness is taken from the *PART definition. LT.0: User-defined (Fabric) thickness. The fabric thickness is set to |THKF|. A1 Viscous coefficient for the porous flow Ergun equation . GT.0: For CTYPE = 11 which is the coefficient for normal-to-segment direction. A1 = 𝐴𝑛 For CTYPE = 12 A1 = 𝐴𝑥 which is the coefficient for the x-direction in the coordinate system specified by DIREC. LT.0: If POREINI = 0.0, the coefficient is time dependent through a load curve id defined by |A1|. If POREI- NI > 0.0, the coefficient is porosity dependent through a load curve id defined by |A1|. The porosity is defined by PORE . B1 Inertial coefficient for the porous flow Ergun equation . GT.0: For CTYPE = 11 B1 = 𝐵𝑛 VARIABLE DESCRIPTION A2 B2 which is the coefficient for normal-to-segment direction. For CTYPE = 12 B1 = 𝐵𝑥 which is the coefficient for the x-direction of a coordinate system specified by DIREC. LT.0: If POREINI = 0.0, the coefficient is time dependent through a load curve id defined by |B1|. If POREI- NI > 0.0, the coefficient is porosity dependent through a load curve id defined by |B1|. The porosity is defined by PORE . For CTYPE = 12 Viscous coefficient for the porous flow Ergun equation . GT.0: Coefficient for the y-direction of a coordinate systems specified by DIREC. A2 = 𝐴𝑦 LT.0: If POREINI = 0.0, the coefficient is time dependent through a load curve id defined by |A1|. If POREI- NI > 0.0, the coefficient is porosity dependent through a load curve id defined by |A2|. The porosity is defined by PORE . For CTYPE=12 Inertial coefficient for the porous flow Ergun equation . GT.0: Coefficient for the y-direction of a coordinate system specified by DIREC. B2 = 𝐵𝑦 LT.0: If POREINI = 0.0 and B2 < 0, the coefficient is time dependent through a load curve id defined by |B2|. If POREINI > 0.0 and B2 < 0, the coefficient is porosity dependent through a load curve id defined by |B2|. The porosity is defined by PORE . A3 For CTYPE = 12 Viscous coefficient for the porous flow Ergun equation . VARIABLE DESCRIPTION GT.0: Coefficient for the z-direction of a coordinate system specified by DIREC. A3 = 𝐴𝑧 LT.0: If POREINI = 0.0 and A3 < 0, the coefficient is time dependent through a load curve id defined by |A3|. If POREINI > 0.0 and A3 < 0, the coefficient is porosity dependent through a load curve id defined by |A3|. The porosity is defined by PORE . B3 For CTYPE = 12 Inertial coefficient for the porous flow Ergun equation . GT.0: Coefficient for the z-direction of a coordinate system specified by DIREC. B3 = 𝐵𝑧 LT.0: If POREINI = 0.0 and B3 < 0, the coefficient is time dependent through a load curve id defined by |B3|. If POREINI > 0.0 and B3 < 0, the coefficient is porosity dependent through a load curve id defined by |B3|. The porosity is defined by PORE . POREINI For CTYPE = 11 or CTYPE = 12 POREINI is the initial volume of pores in an element. The current volume is PORE = POREINI × 𝑣(𝑡) 𝑣(𝑡0) where 𝑣(𝑡) and 𝑣(𝑡0) are the current and initial element volumes respectively. VENTSID Set ID of the vent hole shape. VENTYP Vent surface area set ID type: EQ.0: Part set ID (PSID). EQ.1: Part ID (PID). EQ.2: Segment set ID (SGSID). VTCOEF Flow coefficient for each vent surface area. VARIABLE POPPRES DESCRIPTION Venting pop pressure limit. If the pressure inside the airbag is lower than this pressure, then nothing is vented. Only when the pressure inside the airbag is greater than POPPRES that venting can begin. COEFLC A time-dependent multiplier load curve for correcting the vent flow coefficient, with values ranging from 0.0 to 1.0. Best Practices: Due to the complexity of this card, some comments on simple, efficient and robust coupling approach are given here. These are not rigid guidelines, but simply some experience-based observations. 1. Definition (Fluid and Structure). The term fluid, in the Fluid-Structure Interaction (FSI), refers to materials with ALE element formulation, not indicat- ing the phase (solid, liquid or gas) of those materials. In fact, solid, liquid and gas can all be modeled by the ALE formulation. The term structure refers to materials with Lagrangian element formulation. 2. Default Values (CTYPE and MCOUP). In general, penalty coupling (CTYPE 4 & 5) is recommended, and MCOUP=negative integer is a better choice to define a specific ALE multi-material group (AMMG) to be coupled to the Lagrangian surface. At the minimum, all parameters on card 1 are to be specified, and the default values for most are good starting choices (except MCOUP). 3. How to Correct Leakage. If there is leakage, PFAC, FRCMIN, NORMTYPE and ILEAK are the 4 parameters that can be adjusted. a) For hard structure (steel) and very compressible fluid (air), PFAC may be set to 0.1 (or higher). PFAC = constant value. b) Next, keeping PFAC = constant and set PFACMM = 3 (optional card 4a). This option scales the penalty factor by the bulk modulus of the Lagrangi- an structure. This new approach has also shown to be effective for some airbag application. c) The next approach may be switching from constant PFAC to a load curve approach (i.e. PFAC = load curve, and PFACMM = 0). By looking at the pressure in the system near leakage original location, we can get a feel for the pressure required to stop it. d) If leakage persists after some iterations on the coupling force controls, one can subsequently try to set ILEAK = 2 in combination with the other con- trols to prevent leakage. e) If the modifications fail to stop the leakage, maybe the meshes have to be redesigned to allow better interactions between the Lagrangian and Ale materials. In the example below, the underlined parameters are usually defined parame- ters. A full card definition is shown for reference. $...|....1....|....2....|....3....|....4....|....5....|....6....|....7....|....8 *CONSTRAINED_LAGRANGE_IN_SOLID $ SLAVE MASTER SSTYP MSTYP NQUAD CTYPE DIREC MCOUP 1 11 0 0 4 4 2 -123 $ START END PFAC FRIC FRCMIN NORM NORMTYPE DAMP 0.0 0.0 0.1 0.00 0.3 0 0 0.0 $ CQ HMIN HMAX ILEAK PLEAK LCIDPOR NVENT IBLOCK 0 0 0 0 0.0 0 0 0 $4A IBOXID IPENCHK INTFORC IALESOF LAGMUL PFACMM THKF $ 0 0 0 0 0 0 0 $4B A1 B1 A2 B2 A3 B3 $ 0.0 0.0 0.0 0.0 0.0 0.0 $4C VNTSID VENTYPE VENTCOEF POPPRES COEFLCID (STYPE:0=PSID;1=PID;2=SGSID) $ 0 0 0 0.0 0 $...|....1....|....2....|....3....|....4....|....5....|....6....|....7....|...8 Remarks: 1. Meshing. In order for a fluid-structure interaction (FSI) to occur, a Lagrangian (structure or slave) mesh must spatially overlap with an ALE (fluid or master) mesh. Each mesh should be defined with independent node IDs. LS-DYNA searches for the spatial intersection of between the Lagrangian and ALE mesh- es. Where the meshes overlap, there is a possibility that interaction may occur. In general, SLAVE, MASTER, SSTYP and MSTYPE are required definitions for specifying overlapping-domains coupling search. 2. Number of Coupling Points. The number of coupling points, NQUAD × NQUAD, is distributed over the surface of each Lagrangian segment. General- ly, 2 or 3 coupling points per each Eulerian/ALE element width is adequate. Consequently, the appropriate NQUAD values must be estimated based on the relative resolutions between the Lagrangian and ALE meshes. For example, if 1 Lagrangian shell element spans 2 ALE elements, Then NQUAD for each Lagrangian segment should be 4 or 6. Alternatively, if 2 or 3 Lagrangian segments span 1 ALE element, then maybe NQUAD = 1 would be adequate. If either mesh compresses or expands during the interaction, the number of coupling points per ALE element will also change. The user must account for this and try to maintain at least 2 coupling points per each ALE element side length during the whole process to prevent leakage. Too many coupling points can result in instability, and not enough can result in leakage. 3. The Constraint Method. The constraint method violates kinetic energy balance. The penalty method is therefore recommended. Historically, CTYPE=2 was sometimes used to couple Lagrangian beam nodes to ALE or Lagrangian solids, e.g., for modeling rebar in concrete, or tire cords in rubber. solids, For *CONSTRAINED_BEAM_IN_SOLID is now preferred. constraint-based coupling beams such in of 4. Coupling Direction. DIREC=2 (compression only) may be generally a more stable and robust choice for coupling direction. However, the physics of the problem should dictate the coupling direction. DIREC=1 couples under both tension and compression. This is sometimes useful; for example, in the case of a suddenly accelerating liquid in a container. DIREC=3 is rarely appropriate because it models an extremely sticky fluid. 5. Multi-material Coupling Option. When MCOUP is a negative integer; for example MCOUP= -123, then an ALE multi-material set-ID (AMMSID) of 123 must exist. This is an ID defined by a *SET_MULTI-MATERIAL_GROUP_LIST card. This generally seems to be a better approach to couple to a specific set of AMMGs, and have a clearly defined fluid interface interacting with a Lagrangi- an surface. That way, any leakage may be visualized and the penalty force can be computed more precisely. The Couple to all materials option as activated by MCOUP = 0 is generally not recommended. LS-DYNA calculates the fluid coupling interface as the surface where the sum of coupled ALE materials occupies a volume fraction (Vf) equal to 50%. Since MCOUP = 0 couples to all materials, the sum of all coupled ALE materials is, in this case, trivially 100%. Consequently, when MCOUP = 0 there will not be a fluid interface with which to track leakage. Shell Shell normal vector Shell normal vector Fluid Fluid & Shell will interact Shell Motion Void Shell Motion Fluid Shell Void Fluid & Shell will not interact, use NORM = 1 to reverse the vector Shell normal vector Shell normal vector Figure 10-32. Shell Motion 6. Normal Vector Direction. The normal vectors (NV) of a Lagrangian shell part are defined by the order of the nodes in *ELEMENT definitions, via the right hand rule, and for a segment set, the order of nodes defined in *SET_SEG- MENT. Let the side pointed to by NV be “positive”. The penalty method measure penetration as the distance the ALE fluid penetrates from the positive side to the negative side of the Lagrangian segment. Only fluid on the positive side will be “seen” and coupled to. Therefore, all normal vectors of the Lagrangian segments should point uniform- ly toward the ALE fluid(s), AMMGs, to be coupled to. If NV point uniformly away from the fluid, coupling is not activated. In this case, coupling can be activated by setting NORM = 1. Sometimes a shell part or mesh is generated such that its normal vectors do not point uniformly in a consistent direction (all toward the inside or outside of a container, etc.) The user should always check for the normal vectors of any Lagrangian shell part interacting with any fluid. The NORM parameter may be used to flip the normal direction of all the seg- ments included in the Lagrangian slave set. See Figure 10-32. 7. Coupling-Damping Factor. The user-input coupling-damping factor (DAMP) is used to scale down the critical-damping force (~ damper constant × velocity). For a mass-to-rigid-wall system connected by a parallel-spring-damper con- nector, we can obtain solution for a critically-damped case. DAMP is a factor for scaling down the amount of damping, with DAMP=1 being a critically- damped case. 8. Heat Transfer. The method used is similar to that done by *CONTACT_…_ THERMAL_… card, except radiation heat transfer is not considered. A gap, 𝑙, is assumed to exist between the 2 materials undergoing heat transfer (one is Lagrangian and the other ALE). The convection heat transfer in the gap is as- sumed to approach simple conduction across the medium in the gap. 𝑞 = 𝐾 𝑑𝑇 𝑑𝑥 ~ℎΔ𝑇 ⇒ ℎ~ The heat flux is typically defined as an energy transfer rate per unit area, 𝑞 ∼ [ 𝐽 𝑠 ⁄ ] 𝑚2 . The constant K is the thermal conductivity of the material in the gap; ℎ, is the equivalent convection heat transfer coefficient; and Δ𝑇 is the tempera- ture difference between the master and slave sides. There are 3 possible scenar- ios: ℎ~ ⎧ { { { { { ⎨ { { { { { ⎩ 𝑙⁄ ⁄ HMIN HMAX < 𝑙 HMIN ≤ 𝑙 ≤ HMAX 0 < 𝑙 < HMIN The ALE fluid must be modelled using the ALE single material with void ele- ment formulation (ELFORM = 12) because the LS-DYNA thermal solver sup- ports only one temperature per node. However, a workaround enables partial support for ELFORM =11. Rather than using the thermal solver’s nodal tem- perature field, the ALE temperature is derived from element’s internal energy using the heat capacity. The heat is then extracted from or added to the internal energy of ALE elements. This feature was implemented to calculate the heat exchange between a gas mixture, modeled with *MAT_GAS_MIXTURE and ALE multi-material formulation ELFORM = 11, and a Lagrangian container. HMIN < 0 turns on constraint-based thermal nodal coupling between the La- grangian surface nodes and ALE fluid nodes. This option only works with ALE single material with void element formulation (ELFORM = 12). Once a Lagran- gian surface node is in contact with ALE fluid (gap = 0), the heat transfer de- scribed above is turned off. Instead the Lagrangian surface node temperature is constrained to the ALE fluid temperature field. 9. Leakage Control. The dominate force preventing leakage across a coupled Lagrangian surface should be the penalty associated with the coupling. Forces from the leakage control algorithm feature should be secondary. The *DATA- BASE_FSI keyword controls the “dbfsi” file, which reports both the coupling forces and the leakage control force contribution. It is useful for debugging and fine-tuning. ILEAK = 2 conserves energy; thus, it is better for airbag applications. Leakage control should only be enabled when (1) coupling to a specific AMMG (MCOUP as a negative integer) is activated, and (2) the fluid interface is clearly defined and tracked through the *ALE_MULTI-MATERIAL_GROUP card. 10. Pressure Definition in Porous Flow. There are currently two methods to model porous flow across a Lagrangian shell structure. Both methods involve defining an empirical data curve of relative porous gas velocity as a function of system pressure. However the pressure definitions are slightly different de- pending on the choice of parameter defined: a) When porous flow is modelled using the LCIDPOR parameter (part of this keyword), the velocity response curve expected to be given in terms of the pressure difference: 𝑃upstream − 𝑃downstream. b) When LCIDPOR is negative, porous flow is modelled using the *MAT_- FABRIC material model. The FAC field in *MAT_FABRIC contains a load curve ID given in terms of absolute upstream pressure, rather than in terms of the pressure difference. The *AIRBAG_ALE keyword assumes that the curve referenced by FAC in *MAT_FABRIC is given in terms of absolute upstream pressure. These absolute pressure data are required for the CV phase. During the ALE phase, LS-DYNA automatically shifts the FAC curve left (negative) by 1 atmospheric pressure for the porous coupling calculation, which uses gauge pressure, rather than abso- lute pressure. The mass flowing across a porous Lagrangian surface can be tracked by the “pleak” parameter of the optional “dbfsi” ASCII output file, which may be enabled with the *DATABASE_FSI keyword. 11. Venting. There are 2 methods to model (airbag) venting. The accumulated mass output of both may be tracked via the *DATABASE_FSI card (“pleak” parameter in the “dbfsi” ASCII output file). a) Isentropic Venting. In isentropic venting, (define NVENT on card 3) the flow crossing the vent hole surface is estimated from the isentropic equa- tion. All airbag shell normal vectors should point uniformly in the same direction: typically, inward. The shell elements for the vent holes, includ- ed in the Lagrangian coupling set, should also point in the same direction as the airbag meaning usually inward. For more details on isentropic venting see *AIRBAG_WANG_NEFSKE mass flow rate equation for op- tion OPT EQ.1 and 2. b) Physical Venting. Physical venting models involve holes in the Lagran- gian structure (usually airbags). The shell parts representing the vent holes may be either excluded from the Lagrangian coupling set, or, if in- cluded, have normal vectors reversed from the rest of the airbag. Typical- ly, this means the holes having outward facing normal vectors, since the rest of the airbag has inward pointing normal vectors. With either ap- proach the holes produce no coupling force to stop fluid leakage. When a particular AMMG is present on both sides of the same Lagrangi- an shell surface, penalty coupling can break down. Therefore, It is rec- ommended that *ALE_FSI_SWITCH_MMG_ID be used to switch the AMMG ID of the vented gas so that the vented gas outside the bag does not lead to leakage. 12. Initial Penetration Check. Typically, penetration check (IPENCHK) should only be used if there is high coupling force applied at t=0. For example, consid- er a Lagrangian container, filled with non-gaseous fluid (i.e. ALE liquid or solid) via the *INITIAL_VOLUME_FRACTON_GEOMETRY command. Some- times due to mesh resolution or complex container geometry, there is initial penetration of the fluid across the container surface. This can give rise to a sharp and immediate coupling force on the fluid at t=0. Turning on IPENCHK may help eliminate this spike in coupling force. 13. Porous Flow for Shell Elements. For shell, CTYPE=11, the Ergun-type empirical porous flow equation is applied to the normal flow direction across the porous surface. The pressure gradient along the segment normal direction is 𝑑𝑃 𝑑𝑥𝑛 = 𝐴𝑛(𝜀, 𝜇)𝑉𝑛 + 𝐵𝑛(𝜀, 𝜌)|𝑉𝑛|𝑉𝑛 where the subscript “n” refers to the direction normal to the porous Lagrangian shell surface and where, a) 𝑉𝑛 is the relative normal-to-porous-shell-surface fluid velocity compo- nent. b) 𝐴𝑛(𝜀, 𝜇) = 𝐴1(𝜀, 𝜇) is a viscous coefficient of the Ergun-type porous flow equation. As applied here it should contain the fluid dynamic viscosity, 𝜇 , and shell porosity, 𝜀 information. c) 𝐵𝑛(𝜀, 𝜌) = 𝐵1(𝜀, 𝜌) is an inertial coefficient of the Ergun-type porous flow equation. As applied here it should contain the fluid density, 𝜌, and shell porosity, 𝜀, information. The force increment applied per segment is 𝐹𝑛 = 𝑑𝜌 𝑑𝑥𝑛 × THKF × 𝑆, N5 N1 N8 Ez N4 Ey Ex N6 N2 N7 N3 Figure 10-33. The Ex direction is aligned along the line segment connecting the centers of the 2-3-6-7 and the 1-4-8-5 faces. The Ey direction is orthogonal to the Ex direction and in the plane containing both Ex and containing the segment connecting the centers of the 1-2-6-5 and 3-4-8-7 faces. The Ez is normal to this plane. where, 𝑆 is the segment surface area. If *DEFINE_POROUS_LAGRANGIAN defines the porous properties of a slave element, the porous forces are computed with an equation similar to the one used in *LOAD_BODY_POROUS NOTE: 𝐴𝑖(𝜀, 𝜇), 𝐵𝑖(𝜀, 𝜌), and THKF are required input for porous shell coupling. 14. Porous Flow for Solid Elements. For porous solid, CTYPE=12, the pressure gradient along each global direction (i) can be computed similarly. 𝑑𝑃 𝑑𝑥𝑖 = 𝐴𝑖(𝜀, 𝜇)𝑉𝑖 + 𝐵𝑖(𝜀, 𝜌)|𝑉𝑖|𝑉𝑖 for 𝑖 = 1,2,3 Where, a) 𝑉𝑖 is the relative fluid velocity component through the porous solid in the 3 global directions. b) 𝐴𝑖(𝜀, 𝜇) is a viscous coefficient of the Ergun-type porous flow equation in the ith direction. As applied here it should contain the fluid dynamic vis- cosity, 𝜇, and shell porosity, 𝜀, information. c) 𝐵𝑖(𝜀, 𝜌) is an inertial coefficient of the Ergun-type porous flow equation in the ith direction. As applied here it should contain the fluid density (𝜌) and solid porosity (𝜀) information. NOTE: 𝐴𝑖(𝜀, 𝜇), and 𝐵𝑖(𝜀, 𝜌) are required input for porous solid coupling. system If DIREC = 1, the pressure gradient in a solid is applied in a local reference coordinate If *DEFINE_POROUS_LAGRANGIAN defines the porous properties of a slave element, the local system can be adapted and the porous forces are computed with an equation similar to the one used in *LOAD_BODY_POROUS. defined Figure 10-33. in *CONSTRAINED_LINEAR_GLOBAL Purpose: Define linear constraint equations between displacements and rotations, which can be defined in global coordinate systems. Card 1 1 2 3 4 5 6 7 8 Variable LCID Type I Default none DOF Card. Define one card for each constrained degree-of-freedom. Input is terminated when a "*" card is found. Card 2 1 2 3 4 5 6 7 8 Variable NID DOF COEF Type I Default none Remark 1 VARIABLE LCID I 0 I 0 DESCRIPTION Linear constraint definition ID. This ID can be used to identify a set to which this constraint is a member. NID Node ID VARIABLE DESCRIPTION DOF Degree of freedom in the global coordinate system; EQ.1: displacement along global 𝑥-direction EQ.2: displacement along global 𝑦-direction EQ.3: displacement along global 𝑧-direction EQ.4: global rotation about global 𝑥-axis EQ.5: global rotation about global 𝑦-axis EQ.6: global rotation about global 𝑧-axis COEF Nonzero coefficient, 𝐶𝑘 Remarks: Nodes of a nodal constraint equation cannot be members of another constraint equation or constraint set that constrain the same degrees-of-freedom, a tied interface, or a rigid body; i.e. nodes cannot be subjected to multiple, independent, and possibly conflicting constraints. Also care must be taken to ensure that single point constraints applied to nodes in a constraint equation do not conflict with the constraint sets constrained degrees-of-freedom. In this section linear constraint equations of the form: ∑ 𝐶𝑘𝑢𝑘 = 𝐶0 𝑘=1 can be defined, where uk are the displacements and Ck are user defined coefficients. Unless LS-DYNA is initialized by linking to an implicit code to satisfy this equation at the beginning of the calculation, the constant C0 is assumed to be zero. The first constrained degree-of-freedom is eliminated from the equations-of-motion: its velocities and accelerations are given by 𝑢1 = 𝐶0 − ∑ 𝑘=2 𝐶𝑘 𝐶1 𝑢𝑘 𝑢̇1 = − ∑ 𝑘=2 𝑢̈1 = − ∑ 𝑘=2 𝐶𝑘 𝐶1 𝐶𝑘 𝐶1 𝑢̇𝑘 𝑢̈𝑘, respectively. In the implementation a transformation matrix, 𝐋, is constructed relating the unconstrained, 𝐮, and constrained, 𝐮𝑐, degrees-of-freedom. The constrained accelerations used in the above equation are given by: 𝐮̈𝑐 = [𝐋T𝐌𝐋]−1𝐋T𝐅 where 𝐌 is the Diagonal lumped mass matrix and 𝐅 is the right hand side force vector. This requires the inversion of the condensed mass matrix which is equal in size to the number of constrained degrees-of-freedom minus one. Example: $$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ $ $$$$ *CONSTRAINED_LINEAR_GLOBAL $ $$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ $ $ Constrain nodes 40 and 42 to move identically in the z-direction. $ $ When the linear constraint equation is applied, it goes like this: $ $ 0 = C40uz40 + C42uz42 $ $ = uz40 - uz42 $ $ uz40 = uz42 $ $ where, $ C40 = 1.00 coefficient for node 40 $ C42 = -1.00 coefficient for node 42 $ uz40 = displacement of node 40 in z-direction $ uz42 = displacement of node 42 in z-direction $ $ *CONSTRAINED_LINEAR $ $...>....1....>....2....>....3....>....4....>....5....>....6....>....7....>....8 $ i $ id 2 $ $ nid dof coef 40 3 1.00 42 3 -1.00 $ $ $$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ $ *CONSTRAINED_LINEAR_LOCAL Purpose: Define linear constraint equations between displacements and rotations, which can be defined in a local coordinate system. Each node may have a unique coordinate ID. Card 1 1 2 3 4 5 6 7 8 Variable LCID Type I Default none DOF Cards. Define one card for each constrained degree-of-freedom. Input is terminated at next “*” card. Card 2 1 2 3 4 5 6 7 8 Variable NID DOF CID COEF Type I Default none Remark 1 VARIABLE LCID I 0 I 0 I 0 DESCRIPTION LCID for linear constraint definition. This ID can be used to identify a set to which this constraint is a member. NID Node ID VARIABLE DESCRIPTION DOF Degree of freedom in the local coordinate system; EQ.1: displacement along local x-direction EQ.2: displacement along local y-direction EQ.3: displacement along local z-direction EQ.4: local rotation about local x-axis EQ.5: local rotation about local y-axis EQ.6: local rotation about local z-axis CID Local coordinate system ID number. If the number is zero, the global coordinate system is used. COEF Nonzero coefficient, Ck Remarks: In this section linear constraint equations of the form: ∑ 𝐶𝑘 𝑘=1 𝐿 = 𝐶0 𝑢𝑘 𝐿 are the displacements in the local coordinate systems and Ck can be defined, where 𝑢𝑘 are user defined coefficients. Unless LS-DYNA is initialized by linking to an implicit code to satisfy this equation at the beginning of the calculation, the constant C0 is assumed to be zero. The first constrained degree-of-freedom is eliminated from the equations-of-motion: Its velocities and accelerations are given by 𝐿 = 𝐶0 − ∑ 𝑢1 𝑘=2 𝐶𝑘 𝐶1 𝐿 𝑢𝑘 𝐿 = − ∑ 𝑢̇1 𝑘=2 𝐿 = − ∑ 𝑢̈1 𝑘=2 𝐶𝑘 𝐶1 𝐶𝑘 𝐶1 𝑢̇𝑘 𝑢̈𝑘 respectively. The local displacements are calculated every time step using the local coordinate systems defined by the user. More than one degree of freedom for a node can be constrained by specifying a card for each degree of freedom. WARNING: Nodes of a nodal constraint equation cannot be mem- bers of another constraint equation or constraint set that contains the same degrees-of-freedom, tied inter- face, or rigid bodies. Nodes must not be subject to multiple, independent, and possibly conflicting constraints. Furthermore, care must be taken to ensure that single point con- straints applied to nodes in a constraint equation do not conflict with the constraint set’s constrained de- grees-of-freedom. Purpose: Define a local boundary constraint plane. *CONSTRAINED Card 1 Variable Type Default 1 TC 1 0 2 RC 1 0 3 DIR 1 0 4 X F 0 5 Y F 0 8 6 Z F 0 7 CID 1 none VARIABLE DESCRIPTION TC Translational Constraint in local system: EQ.1: constrained x translation, EQ.2: constrained y translation, EQ.3: constrained z translation, EQ.4: constrained x and y translations, EQ.5: constrained y and z translations, EQ.6: constrained x and z translations, EQ.7: constrained x, y, and translations. RC Rotational Constraint in local system: EQ.1: constrained x-rotation, EQ.2: constrained y-rotation, EQ.3: constrained z-rotation, EQ.4: constrained x and y rotations, EQ.5: constrained y and z rotations, EQ.6: constrained z and x rotations, EQ.7: constrained x, y, and z rotations. VARIABLE DESCRIPTION DIR Direction of normal for local constraint plane. EQ.1: local x, EQ.2: local y, EQ.3: local z. Local x-coordinate of a point on the local constraint plane. Local y-coordinate of a point on the local constraint plane. Local z-coordinate of a point on the local constraint plane. Coordinate system ID for orientation of the local coordinate system. X Y Z CID Remarks: Nodes within a mesh-size-dependent tolerance are constrained on a local plane. This option is recommended for use with r-method adaptive remeshing where nodal constraints are lost during the remeshing phase. *CONSTRAINED_MULTIPLE_GLOBAL Purpose: Define global multi-point constraints for imposing periodic boundary condition in displacement field. 2 3 4 5 6 7 8 Card 1 Variable 1 ID Type I Default NOTE: For each constraint equation include a set of cards consisting of (1) a Constraint Equation Definition Card and (2) NMP Coefficient Cards. Constraint Equation Definition Card. Card 2 1 2 3 4 5 6 7 8 Variable NMP Type I Default Coefficient Cards. The next NMP cards adhere to this format. Each card sets a single coefficient in the constraint equation. Card 3 1 2 3 4 5 6 7 8 Variable NID DIR COEF Type I I F Default 11 8 5 7 4 *CONSTRAINED_MULTIPLE_GLOBAL 9 6 1 3 3, 1, 1.0 1, 1,-1.0 10 10, 1,-1.0 (3) − 𝑢1 𝑢1 (1) − 𝑢1 (10) = 0 1 2 3 3 8, 1, 1.0 2, 1,-1.0 11, 1,-1.0 (8) − 𝑢1 𝑢1 (2) − 𝑢1 (11) = 0 *CONSTRAINED_MULTIPLE_GLOBAL 2 3 3, 2, 1.0 1, 2,-1.0 10, 2,-1.0 (3) − 𝑢2 𝑢2 (1) − 𝑢2 (10) = 0 Figure 10-34. Simple example. VARIABLE DESCRIPTION ID Constraint set identification. All constraint sets should have a unique set ID. NMP Number of nodes to be constrained mutually. NID DIR Nodal ID Direction in three-dimensional space to be constrained EQ.1: 𝑥 direction EQ.2: 𝑦 direction EQ.3: 𝑧 direction LT.0: Extra DOFs for user defined element formulation (e.g. - 1: the 1st extra DOF; -2: the 2nd extra DOF; …) VARIABLE DESCRIPTION COEF Coefficient 𝛼NID in constraint equation: ∑ 𝛼NID𝑢DIR NID (NID) = 0 . Remarks: 1. Defining multi-point constraints by this keyword can be demonstrated by the following example: a two-dimensional unit square with four quadrilateral ele- ments and 11 nodes as shown in the figure below, where the nodes #10 and #11 are two dummy nodes serving as control points. *CONSTRAINED_NODAL_RIGID_BODY_{OPTION}_{OPTION}_{OPTION} Available options include: <BLANK> SPC INERTIA TITLE If the center of mass is constrained use the SPC option. If the inertial properties are defined rather than computed use the INERTIA option. A description for the nodal rigid body can be defined with the TITLE option. Purpose: Define a nodal rigid body. This is a rigid body which consists of the defined nodes. If the INERTIA option is not used, then the inertia tensor is computed from the nodal masses. Arbitrary motion of this rigid body is allowed. If the INERTIA option is used, constant translational and rotational velocities can be defined in a global or local coordinate system. The first node in the nodal rigid body definition is treated as the master for the case where DRFLAG and RRFLAG are nonzero. The first node always has six degrees-of- freedom. The release conditions applied in the global system are sometimes convenient in small displacement linear analysis, but, otherwise, are not recommended. It is strongly recommended, especially for implicit calculations, that release conditions are only used for a two noded nodal rigid body. Card Format: Card 1: required Card 2: required for SPC option Card 3 - 5: required for INERTIA option Card 6: required if a local coordinate system is used to specify the inertia tensor when the INERTIA option is set Remarks: 1. Unlike the *CONSTRAINED_NODE_SET which permits only constraints on translational motion, here the equations of rigid body dynamics are used to update the motion of the nodes and therefore rotations of the nodal sets are admissible. Mass properties are determined from the nodal masses and coor- dinates. Inertial properties are defined if and only if the INERTIA option is specified. Title Card. Additional card for the TITLE keyword option. Optional 1 2 3 4 5 6 7 8 Variable Type TITLE A80 Card 1 1 2 3 4 5 6 7 8 Variable PID CID NSID PNODE IPRT DRFLAG RRFLAG Type I I I Default none none none I 0 I 0 I 0 I 0 Center of Mass Constraint Card. Additional card for the SPC keyword option. Card 2 1 2 3 4 5 6 7 8 Variable CMO CON1 CON2 Type Default F 0 F 0 F 0 VARIABLE DESCRIPTION PID CID Part ID of the nodal rigid body. Optional coordinate system ID for the rigid body local system, see *DEFINE_COORDINATE_OPTION. Output of the rigid body data and the degree-of- freedom releases are done in this local system. This local system rotates with the rigid body. VARIABLE NSID PNODE DESCRIPTION Nodal set ID, see *SET_NODE_OPTION. This nodal set defines the rigid body. If NSID = 0, then NSID = PID, i.e., the node set ID and the part ID are assumed to be identical. An optional node (a massless node is allowed) used for post processing rigid body data. If the PNODE is not located at the rigid body’s center of mass, then the initial coordinates of PNODE will be reset to the center of mass. If CID is defined, the velocities and accelerations of PNODE will be output in the local system to the d3plot and d3thdt files unless PNODE is specified as a negative number, in which case the global system is used. IPRT Print flag. For nodal rigid bodies the following values apply: EQ.1: write data into rbdout EQ.2: do not write data into rbdout Printing is suppressed for two noded rigid bodies unless IPRT is set to unity. This is to avoid excessively large rbdout files when many, two-noded welds are used. DRFLAG Displacement release flag for all nodes except the first node in the definition. EQ.-7: release 𝑥, 𝑦, and 𝑧 displacement in global system EQ.-6: release 𝑧 and 𝑥 displacement in global system EQ.-5: release 𝑦 and 𝑧 displacement in global system EQ.-4: release 𝑥 and 𝑦 displacement in global system EQ.-3: release 𝑧 displacement in global system EQ.-2: release 𝑦 displacement in global system EQ.-1: release 𝑥 displacement in global system EQ.0: off for rigid body behavior EQ.1: release 𝑥 displacement in rigid body local system EQ.2: release 𝑦 displacement in rigid body local system EQ.3: release 𝑧 displacement in rigid body local system EQ.4: release 𝑥 and 𝑦 displacement in rigid body local system EQ.5: release 𝑦 and 𝑧 displacement in rigid body local system EQ.6: release 𝑧 and 𝑥 displacement in rigid body local system EQ.7: release 𝑥, 𝑦, and 𝑧 displacement in rigid body local VARIABLE DESCRIPTION system RRFLAG Rotation release flag for all nodes except the first node in the definition. EQ.-7: release 𝑥, 𝑦, and 𝑧 rotations in global system EQ.-6: release 𝑧 and 𝑥 rotations in global system EQ.-5: release 𝑦 and 𝑧 rotations in global system EQ.-4: release 𝑥 and 𝑦 rotations in global system EQ.-3: release 𝑧 rotation in global system EQ.-2: release 𝑦 rotation in global system EQ.-1: release 𝑥 rotation in global system EQ.0: off for rigid body behavior EQ.1: release 𝑥 rotation in rigid body local system EQ.2: release 𝑦 rotation in rigid body local system EQ.3: release 𝑧 rotation in rigid body local system EQ.4: release 𝑥 and 𝑦 rotations in rigid body local system EQ.5: release 𝑦 and 𝑧 rotations in rigid body local system EQ.6: release 𝑧 and 𝑥 rotations in rigid body local system EQ.7: release 𝑥, 𝑦, and 𝑧 rotations in rigid body local system CMO Center of mass constraint option, CMO: EQ.+1.0: constraints applied in global directions, EQ.0.0: no constraints, EQ.-1.0: constraints applied constraint). in local directions (SPC CON1 First constraint parameter: If CMO=+1.0, then specify global translational constraint: EQ.0: no constraints, EQ.1: constrained 𝑥 displacement, EQ.2: constrained 𝑦 displacement, EQ.3: constrained 𝑧 displacement, EQ.4: constrained 𝑥 and 𝑦 displacements, VARIABLE DESCRIPTION EQ.5: constrained 𝑦 and 𝑧 displacements, EQ.6: constrained 𝑧 and 𝑥 displacements, EQ.7: constrained 𝑥, 𝑦, and 𝑧 displacements. If CM0 = -1.0, then specify local coordinate system ID. See *DE- FINE_COORDINATE_OPTION: This coordinate system is fixed in time CON2 Second constraint parameter: If CMO=+1.0, then specify global rotational constraint: EQ.0: no constraints, EQ.1: constrained 𝑥 rotation, EQ.2: constrained 𝑦 rotation, EQ.3: constrained 𝑧 rotation, EQ.4: constrained 𝑥 and 𝑦 rotations, EQ.5: constrained 𝑦 and 𝑧 rotations, EQ.6: constrained 𝑧 and 𝑥 rotations, EQ.7: constrained 𝑥, 𝑦, and 𝑧 rotations. If CM0 = -1.0, then specify local (SPC) constraint: EQ.000000: no constraint, EQ.100000: constrained 𝑥 translation, EQ.010000: constrained 𝑦 translation, EQ.001000: constrained 𝑧 translation, EQ.000100: constrained 𝑥 rotation, EQ.000010 : constrained 𝑦 rotation, EQ.000001: constrained 𝑧 rotation. Any combination of local constraints can be achieved by adding the number 1 into the corresponding column. Inertia Card 1. Additional card for the INERTIA keyword option. Card 3 Variable Type Default 1 XC F 0 2 YC F 0 3 ZC F 0 4 TM F 0 5 6 7 8 IRCS NODEID I 0 I 0 VARIABLE DESCRIPTION XC YC ZC TM 𝑥-coordinate of center of mass. If nodal point, NODEID, is defined, XC, YC, and ZC are ignored and the coordinates of the nodal point, NODEID, are taken as the center of mass. 𝑦-coordinate of center of mass 𝑧-coordinate of center of mass Translational mass IRCS Flag for inertia tensor reference coordinate system: EQ.0: global inertia tensor, EQ.1: local inertia tensor is given in a system defined by the orientation vectors as given below. NODEID Optional nodal point defining the CG of the rigid body. If this node is not a member of the set NSID above, its motion will not be updated to correspond with the nodal rigid body after the calculation begins. PNODE and NODEID can be identical if and only if PNODE physically lies at the mass center at time zero. Inertia Card 2. Second Additional card for the INERTIA keyword option. Card 4 1 Variable IXX Type F Default none 2 IXY F 0 3 IXZ F 0 4 IYY F none 5 IYZ F 0 6 IZZ F 0 7 8 VARIABLE DESCRIPTION IXX IXY IXZ IYY IYZ IZZ 𝐼𝑥𝑥, 𝑥𝑥 component of inertia tensor 𝐼𝑥𝑦, 𝑥𝑦 component of inertia tensor 𝐼𝑥𝑧, 𝑥𝑧 component of inertia tensor 𝐼𝑦𝑦, 𝑦𝑦 component of inertia tensor 𝐼𝑦𝑧, 𝑦𝑧 component of inertia tensor 𝐼𝑧𝑧, 𝑧𝑧 component of inertia tensor Inertia Card 3. Third additional card for the INERTIA keyword option. Card 5 1 2 3 4 5 6 7 8 Variable VTX VTY VTZ VRX VRY VRZ Type Default F 0 F 0 F 0 F 0 F 0 F 0 VARIABLE DESCRIPTION VTX VTY 𝑥-rigid body initial translational velocity in global coordinate system. 𝑦-rigid body initial translational velocity in global coordinate system. VARIABLE DESCRIPTION VTZ VRX VRY 𝑧-rigid body initial translational velocity in global coordinate system. 𝑥-rigid body initial rotational velocity in global coordinate system. 𝑦-rigid body initial rotational velocity in global coordinate system. VRZ 𝑧-rigid body initial rotational velocity in global coordinate system. Remarks: The velocities defined above can be overwritten by the *INITIAL_VELOCITY card. Local Inertia Tensor Card. Additional card required for IRCS = 1 . Define two local vectors or a local coordinate system ID. Card 6 Variable 1 XL Type F 2 YL F 3 ZL F 4 5 6 7 8 XLIP YLIP ZLIP CID2 F F F I Default none none none none none none none VARIABLE DESCRIPTION XL YL ZL XLIP YLIP ZLIP CID2 𝑥-coordinate of local 𝑥-axis. Origin lies at (0,0,0). 𝑦-coordinate of local 𝑥-axis 𝑧-coordinate of local 𝑥-axis 𝑥-coordinate of local in-plane vector 𝑦-coordinate of local in-plane vector 𝑧-coordinate of local in-plane vector Local coordinate system ID, see *DEFINE_COORDINATE_.... With this option leave fields 1-6 blank. Remarks: The local coordinate system is set up in the following way. After the local x-axis is defined, the local 𝑧-axis is computed from the cross-product of the local 𝑥-axis vector with the given in-plane vector. Finally, the local 𝑦-axis is determined from the cross- product of the local 𝑧-axis with the local 𝑥-axis. The local coordinate system defined by CID has the advantage that the local system can be defined by nodes in the rigid body which makes repositioning of the rigid body in a preprocessor much easier since the local system moves with the nodal points. Example: $$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ $ $$$$ *CONSTRAINED_NODAL_RIGID_BODY $ $$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ $ $ Define a rigid body consisting of the nodes in nodal set 61. $ $ This particular example was used to connect three separate deformable $ parts. Physically, these parts were welded together. Modeling wise, $ however, this joint is quit messy and is most conveniently modeled $ by making a rigid body using several of the nodes in the area. Physically, $ this joint was so strong that weld failure was never of concern. $ *CONSTRAINED_NODAL_RIGID_BODY $ $...>....1....>....2....>....3....>....4....>....5....>....6....>....7....>....8 $ pid cid nsid 45 61 $ $ nsid = 61 nodal set ID number, requires a *SET_NODE_option $ cid not used in this example, output will be in global coordinates $ $ *SET_NODE_LIST $ sid 61 $ nid1 nid2 nid3 nid4 nid5 nid6 nid7 nid8 823 1057 1174 1931 2124 1961 2101 $ $$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ *CONSTRAINED_NODE_INTERPOLATION Purpose: Define constrained nodes for the use of *ELEMENT_INTERPOLATION_- SHELL and *ELEMENT_INTERPOLATION_SOLID to model contact and to visualize the results of generalized elements . The displacements of these nodes are dependent of their corresponding master nodes. Card 1 1 2 3 4 5 6 7 8 Variable NID NUMMN Type I I Default none none Weighting Factor Cards. For each of the NUMMN master nodes NID depends on set a MN and W entry. Each Weighting Factor Card can accommodate four master nodes. Add as many Weighting Factor Cards as needed. Card 2 1 2 3 4 5 6 7 8 Variable MN1 W1 MN2 W2 MN3 W3 MN4 W4 Type I F I F I F I F Default none none none none none none none none Card 3 1 Variable MN5 2 W5 3 4 5 6 7 8 Etc. Etc. Etc. Etc. Etc. Etc. Type I F I F I F I F Default none none none none none none none none 26 25 24 15 14 16 26 25 78 16 15 Connectivity of Generalized-Shell Element Generalized-Shell Element (*ELEMENT_GENERALIZED_SHELL) Interpolation Node (*CONSTRAINED_NODE_INTERPOLATION) Interpolation Element (*ELEMENT_INTERPOLATION_SHELL) *CONSTRAINED_NODE_INTERPOLATION $---+--NID----+NUMCN----+----3----+----4----+----5----+----6----+----7----+----8 78 $---+--CN1----+---W1----+--CN2----+---W2----+--CN3----+---W3----+--CN4----+---W4 0.15 0.32 0.18 0.35 26 25 16 15 Figure 10-35. Example of a *CONSTRAINED_NODE_INTERPOLATION card VARIABLE NID DESCRIPTION Node ID of the interpolation node as defined in *NODE . NUMMN Number of master nodes, this constrained node depends on. Node ID of master node i. Weighting factor of master node i. MNi Wi Remarks: 1. The coordinates of an interpolation node have to be defined in *NODE. In there the translational and rotational constraints TC = 7. and RC = 7. need to be set. 2. The displacements of the interpolation node, 𝒅IN, are interpolated based on the displacements of the corresponding master nodes, 𝒅𝑖, and the appropriate weighting factors 𝑤𝑖. The interpolation is computed as follows: NUMMN 𝒅IN = ∑ 𝑤𝑖𝒅𝑖 𝑖=1 . *CONSTRAINED_NODE_SET_{OPTION} To define an ID for the constrained node set the following option is available: <BLANK> ID If the ID is defined an additional card is required. Purpose: Define nodal constraint sets for translational motion in global coordinates. No rotational coupling. See Figure 10-36. Nodal points included in the sets should not be subjected to any other constraints including prescribed motion, e.g., with the *BOUNDARY_PRESCRIBED_MOTION options. ID Card. Additional card for ID keyword option. Card 1 1 2 3 4 5 6 7 8 Variable CNSID Type Default I 0 Card 2 1 2 Variable NSID DOF Type I I 3 TF F Default none none 1.E+20 Remarks 1 2 4 5 6 7 8 VARIABLE DESCRIPTION CNSID Optional constrained node set ID. NSID Nodal set ID, see *SET_NODE_OPTION. Since no rotation is permitted, this option should not be used to model rigid body behavior involving rotations *CONSTRAINED_NODE_SET *CONSTRAINED_NODAL_RIGID_BODY *CONSTRAINED_SPOTWELD Behavior is like a rigid beam. These options may be used to model spotwelds. Figure 10-36. Two different ways to constrain node 𝑎 and 𝑏. For rigid-body type situations this card, *CONSTRAINED_NODE_SET may lead to un- physical results. VARIABLE DESCRIPTION DOF Applicable degrees-of-freedom: EQ.1: x-translational degree-of-freedom, EQ.2: y-translational degree-of-freedom, EQ.3: z-translational degree-of-freedom, EQ.4: x and y-translational degrees-of-freedom, EQ.5: y and z-translational degrees-of-freedom, EQ.6: z and x-translational degrees-of-freedom, EQ.7: x, y, and z-translational degrees-of-freedom. TF Failure time for nodal constraint set. Remarks: 1. The masses of the nodes are summed up to determine the total mass of the constrained set. It must be noted that the definition of a nodal rigid body is not possible with this input For nodal rigid bodies the keyword input: *CON- STRAINED_NODAL_RIGID_BODY_OPTION, must be used. 2. When the failure time, TF, is reached the nodal constraint becomes inactive and the constrained nodes may move freely. Example: $$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ $ $$$$ *CONSTRAINED_NODE_SET $ $$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ $ $ Constrain all the nodes in a nodal set to move equivalently $ in the z-direction. $ *CONSTRAINED_NODE_SET $ $...>....1....>....2....>....3....>....4....>....5....>....6....>....7....>....8 nsid dof tf 7 3 10.0 $ $ nsid = 7 nodal set ID number, requires a *SET_NODE_option $ dof = 3 nodal motions are equivalent in z-translation $ tf = 3 at time=10. the nodal constraint is removed $ $$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ $ *CONSTRAINED_NODE_TO_NURBS_PATCH_{OPTION} Purpose: To add additional massless nodes to the surface of a NURBS patch. The motion of the nodes is governed by the NURBS patch. Forces applied to the nodes are distributed to the NURBS patch. Penalty method is used to handle the displacement boundary conditions CON on the specified nodes. To specify node sets instead of individual nodes use the option: SET 6 7 8 Card 1 1 2 3 4 Variable PATCHID NSID CON CID Type I I Default none none I I 0 5 SF F 1.0 VARIABLE DESCRIPTION PATCHID Patch ID. NSID CON CID SF Nodal set ID or node ID depending on the OPTION. Constraint parameter for extra node(s) of NSID. Its definition is in same as that of CON2 when CM0 = -1 as described MAT_RIGID. For example “1110” means constrained 𝑧- translation, 𝑥-rotation and 𝑦-rotation. Coordinate system ID for constraint Penalty force scale factor for the penalty-based constraint *CONSTRAINED Purpose: Constrain two points with the specified coordinates connecting two shell elements at locations other than nodal points. In this option, the penalty method is used to constrain the translational and rotational degrees-of-freedom of the points. Force resultants are written into the swforc ASCII file for post-processing. Card 1 1 2 3 4 5 6 7 8 Variable CID Type I Default none Card 2 1 2 3 4 5 6 7 8 9 10 Variable EID1 Type I Default none X1 F 0. Y1 F 0. Z1 F 0. Card 3 1 2 3 4 5 6 7 8 9 10 Variable EID2 Type I Default none X2 F 0. Y2 F 0. Z2 F 0. Card 4 1 2 3 4 5 6 7 8 Variable PSF FAILA FAILS FAILM Type F F F F Default 1.0 0.0 0.0 0.0 VARIABLE DESCRIPTION CID EIDi Constrained points ID. Shell element ID, i = 1, 2. Xi, Yi, Zi Coordinates of the constrained points, i = 1, 2. PSF Penalty scale factor (Default = 1.0). FAILA Axial force resultant failure value, no failure if zero. FAILS Shear force resultant failure value, no failure if zero. FAILM Moment resultant failure value, no failure if zero. *CONSTRAINED_RIGID_BODIES Purpose: Merge two rigid bodies. One rigid body, called slave rigid body, is merged to the other one called a master rigid body. This command applies to parts comprised of *MAT_RIGID bodies (*CONSTRAINED_NODAL_RIGID_BODY). nodal rigid but not to Card 1 1 2 3 4 5 6 7 8 Variable PIDM PIDS IFLAG Type I I Default none none I 0 VARIABLE DESCRIPTION PIDM PIDS IFLAG Master rigid body part ID, see *PART. Slave rigid body part ID, see *PART. This flag is meaningful if and only if the inertia properties of the Part, PIDM, are defined in PART_INERTIA. EQ.1: Update the center-of-gravity, the translational mass, and the inertia matrix of PIDM to reflect its merging with the slave rigid body (PIDS). EQ.0: The merged PIDS will not affect the properties defined in PART_INERTIA for PIDM since it is assumed the prop- erties already account for merged parts. The inertia properties of PIDS will be computed from its nodal masses if the properties are not defined in a PART_IN- ERTIA definition. Remarks: 1. The slave rigid body is merged to the master rigid body. The inertial properties computed by LS-DYNA are based on the combination of the master rigid body plus all the rigid bodies which are slaved to it unless the inertial properties of the master rigid body are defined via the *PART_INERTIA keyword in which case those properties are used for the combination of the master and slave rigid bodies. Note that a master rigid body may have many slaves. 2. 3. Independent rigid bodies must not share common nodes since each rigid body updates the motion of its nodes independently of the other rigid bodies. If common nodes exist between rigid bodies the rigid bodies sharing the nodes must be merged. It is also possible to merge rigid bodies that are completely separated and share no common nodal points or boundaries. All actions valid for the master rigid body, e.g., constraints, given velocity, are now also valid for the newly-created rigid body. Example: $$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ $ $$$$ *CONSTRAINED_RIGID_BODIES $ $$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ $ $ Rigidly connect parts 35, 70, 71, and 72 to part 12. $ All parts must be defined as rigid. $ $ This example is used to make a single rigid body out of the five parts $ that compose the back end of a vehicle. This was done to save cpu time $ and was determined to be valid because the application was a frontal $ impact with insignificant rear end deformations. (The cpu time saved $ was from making the parts rigid, not from merging them - merging was $ more of a convenience in this case for post processing, for checking $ inertial properties, and for joining the parts.) $ *CONSTRAINED_RIGID_BODIES $...>....1....>....2....>....3....>....4....>....5....>....6....>....7....>....8 $ pidm pids 12 35 12 70 12 71 12 72 $ $$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ *CONSTRAINED_RIGID_BODY_INSERT Purpose: This keyword is for modeling die inserts. One rigid body, called slave rigid body, is constrained to move with another rigid body, called the master rigid body, in all directions except for one. Card 1 Variable 1 ID 2 3 4 5 6 7 8 PIDM PIDS COORDID IDIR Type I I I I Default none none none none Card 2 1 2 3 4 Variable MFLAG MCID DEATHM I 3 5 6 7 8 F 0.0 3 4 5 6 7 8 Type Default I 0 Card 3 1 I 0 2 Variable PARTB DEATHB Type Default I 0 F 0.0 VARIABLE DESCRIPTION ID PIDM PIDS Insert ID Master (die) rigid body part ID, see *PART. Slave (die insert) rigid body part ID, see *PART. VARIABLE COORDID DESCRIPTION Coordinate ID. The 𝑥 direction is the direction the insert moves independently of the die. IDIR The direction the insert moves independently of the die. If unspecified, it defaults to the local z direction, IDIR = 3. MFLAG Motion flag. EQ.0: Relative motion is unconstrained. EQ.1: The displacement of the insert relative to the die is imposed. EQ.2: The velocity of the insert relative to the die is imposed. EQ.3: The acceleration of the insert relative to the die is imposed. MCID Curve defining the motion of the die insert relative to the die. DEATHM Death time of the imposed motion. If it is equal to 0.0, the motion is imposed for the entire analysis. PARTB Part ID for a discrete beam connected between the insert and die. DEATHB Death time for the discrete beam specified by BPART. Remarks: 1. This capability is supported by both the implicit and explicit time integrators; however, the joint death time DEATHM feature works only for explicit integra- tion with the penalty method. 2. The translational joint constraining the die and the die insert are automatically generated. The joint reaction forces will appear in the jntforc output file. 3. The translational motor constraining the remaining translational degree of freedom is also automatically generated, and its reaction forces also appear in the jntforc output file. 4. The automatically generated beam has its data written to the d3plot file, and all of the optional appropriate output files. *CONSTRAINED_RIGID_BODY_STOPPERS Purpose: Rigid body stoppers provide a convenient way of controlling the motion of rigid tooling in metalforming applications. The motion of a “master” rigid body is limited by load curves. This option will stop the motion based on a time dependent constraint. The stopper overrides prescribed motion boundary conditions (except relative displacement) operating in the same direction for both the master and slaved rigid bodies. See Figure 10-37. Card 1 1 2 3 4 5 6 7 Variable PID LCMAX LCMIN PSIDMX PSIDMN LCVMNX DIR 8 VID I 0 3 I 0 4 I 0 5 I I I 0 required 0 6 7 8 Type I I Default required 0 Card 2 Variable Type Default 1 TB F 0 2 TD F 1021 VARIABLE DESCRIPTION PID Part ID of master rigid body, see *PART. LCMAX Load curve ID defining the maximum coordinate or displacement as a function of time. See *DEFINE_CURVE: LT.0: Load Curve ID |LCMAX| provides an upper bound for the displacement of the rigid body EQ.0: no limitation of the maximum displacement. GT.0: Load Curve ID LCMAX provides an upper bound for the position of the rigid body center of mass Slave2 C.G. Slave 1 C.G. Master C.G. D1 D2 Rigid Body Stopper Figure 10-37. When the master rigid body reaches the rigid body stopper, the velocity component into the stopper is set to zero. Slave rigid bodies 1 and 2 also stop if the distance between their mass centers and the master rigid body is less than or equal to the input values D1 and D2, respectively. VARIABLE LCMIN PSIDMX DESCRIPTION Load curve ID defining the minimum coordinate or displacement as a function of time. See *DEFINE_CURVE: LT.0: Load Curve ID |LCMIN| defines a lower bound for the displacement of the rigid body EQ.0: no limitation of the minimum displacement. GT.0: Load Curve ID LCMIN defines a lower bound for the position of the rigid body center of mass Optional part set ID of rigid bodies that are slaved in the maximum coordinate direction to the master rigid body. The part set definition, may be used to define the closure distance (D1 and D2 in Figure 10-37) which activates the constraint. The constraint does not begin to act until the master rigid body stops. If the distance between the master rigid body is greater than or equal to the closure distance, the slave rigid body motion away from the master rigid body also stops. However, the slaved rigid body is free to move towards the VARIABLE DESCRIPTION PSIDMN master. If the closure distance is input as zero (0.0) then the slaved rigid body stops when the master stops. Optional part set ID of rigid bodies that are slaved in the minimum coordinate direction to the master rigid body. The part set definition, may be used to define the closure distance (D1 and D2 in Figure 10-37) which activates the constraint. The constraint does not begin to act until the master rigid body stops. If the distance between the master rigid body is less than or equal to the closure distance, the slave rigid body motion towards the master rigid body also stops. However, the slaved rigid body is free to move away from the master. If the closure distance is input as zero (0.0) then the slaved rigid body stops when the master stops. LCVMX Load curve ID which defines the maximum absolute value of the velocity as a function of time that is allowed for the master rigid body. See *DEFINE_CURVE: EQ.0: no limitation on the velocity. DIR Direction stopper acts in: EQ.1: x-translation, EQ.2: y-translation, EQ.3: z-translation, EQ.4: arbitrary, defined by vector VID , EQ.5: x-axis rotation, EQ.6: y-axis rotation, EQ.7: z-axis rotation, EQ.8: arbitrary, defined by vector VID . Vector for arbitrary orientation of stopper, see *DEFINE_VEC- TOR. Time at which stopper is activated. Time at which stopper is deactivated. VID TB TD Remarks: The optional definition of part sets in minimum or maximum coordinate direction allows the motion to be controlled in arbitrary direction. *CONSTRAINED_RIVET_{OPTION} To define an ID for the rivet, the following option is available: <BLANK> ID If the ID is defined an additional card is required. Purpose: Define massless rivets between non-contiguous nodal pairs. The nodes must not have the same coordinates. The action is such that the distance between the two nodes is kept constant throughout any motion. No failure can be specified. ID Card. Additional card for the ID keyword option. ID 1 2 3 4 5 6 7 8 Variable RID Type Default Card 1 Variable I 0 1 N1 Type I 2 N2 I 3 TF F 4 5 6 7 8 Default none none 1.E+20 Remarks 1 2 VARIABLE DESCRIPTION RID N1 N2 Optional rivet ID. Node ID Node ID VARIABLE DESCRIPTION TF Failure time for nodal constraint set. Remarks: 1. Nodes connected by a rivet cannot be members of another constraint set that constrain the same degrees-of-freedom, a tied interface, or a rigid body, i.e., nodes cannot be subjected to multiple, independent, and possibly conflicting constraints. Also care must be taken to ensure that single point constraints applied to nodes in a constraint set do not conflict with the constraint sets con- strained degrees-of-freedom. 2. When the failure time, TF, is reached the rivet becomes inactive and the constrained nodes may move freely. Example: $$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ $ $$$$ *CONSTRAINED_RIVET $ $$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ $ $ Connect node 382 to node 88471 with a massless rivet. $ *CONSTRAINED_RIVET $ $...>....1....>....2....>....3....>....4....>....5....>....6....>....7....>....8 $ n1 n2 tf 382 88471 0.0 $ $$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ *CONSTRAINED_SHELL_TO_SOLID Purpose: Define a tie between a shell edge and solid elements. Nodal rigid bodies can perform the same function and may also be used. Card 1 1 2 3 4 5 6 7 8 Variable NID NSID Type I I Default none none VARIABLE DESCRIPTION Shell node ID Solid nodal set ID, see *SET_NODE_OPTION. NID NSID Remarks: The shell-brick interface, an extension of the tied surface capability, ties regions of hexahedron elements to regions of shell elements. A shell node may be tied to up to Nodes are constrained to stay on fiber vector. n1 n2 n3 n4 n5 s3 Nodes s1 and n3 are coincident. Figure 10-38. The interface between shell elements and solids ties shell node s1 to a line of nodes on the solid elements n1-n5. It is very important for the nodes to be aligned. nine brick nodes lying along the tangent vector to the nodal fiber. See Figure 10-38. During the calculation, the brick nodes thus constrained, must lie along the fiber but can move relative to each other in the fiber direction. The shell node stays on the fiber at the same relative spacing between the first and last brick node. The brick nodes must be input in the order in which they occur, in either the plus or minus direction, as one moves along the shell node fiber. This feature is intended to tie four node shells to eight node shells or solids; it is not intended for tying eight node shells to eight node solids. Example: $$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ $ $$$$ *CONSTRAINED_SHELL_TO_SOLID $ $$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ $ $ Tie shell element, at node 329, to a solid element at node 203. $ - nodes 329 and 203 are coincident $ $ Additionally, define a line of nodes on the solids elements, containing $ node 203, that must remain in the same direction as the fiber of the shell $ containing node 329. In other words: $ $ - Nodes 119, 161, 203, 245 and 287 are nodes on a solid part that $ define a line on that solid part. $ - This line of nodes will be constrained to remain linear throughout $ the simulation. $ - The direction of this line will be kept the same as the fiber of the $ of the shell containing node 329. $ *CONSTRAINED_SHELL_TO_SOLID $...>....1....>....2....>....3....>....4....>....5....>....6....>....7....>....8 $ nid nsid 329 4 $ *SET_NODE_LIST $ sid 4 $ nid1 nid2 nid3 nid4 nid5 nid6 nid7 nid8 119 161 203 245 287 $ $$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ *CONSTRAINED Purpose: Define an elastic cubic spline interpolation constraint. The displacements and slopes at the end points are continuous. The first and last nodes, which define the constraint, must be independent. The degrees-of-freedom of interior nodes may be either dependent or independent. Card 1 1 2 3 4 5 6 7 8 Variable SPLID DLRATIO Type Default I 0 I 0.10 Node Cards. Include one card per independent/dependent node. The first and last nodes must be independent. The next “*” card terminates this input. Card 2 1 2 3 4 5 6 7 8 Variable NID DOF Type Default I 0 I 0 VARIABLE DESCRIPTION SPLID Spline constraint ID. DLRATIO NID Ratio of bending to torsional stiffness for an elastic tubular beam which connects the independent degrees-of-freedom. The default value is set to 0.10. Independent/dependent node ID. For explicit problems this node should not be a member of a rigid body, or elsewhere constrained in the input. VARIABLE DOF DESCRIPTION Degrees-of-freedom. The list of dependent degrees-of-freedom consists of a number with up to six digits, with each digit representing a degree of freedom. For example, the value 1356 indicates that degrees of freedom 1, 3, 5, and 6 are controlled by the constraint. The default is 123456. Digit: degree of freedom ID's: EQ.1: x EQ.2: y EQ.3: z EQ.4: rotation about x axis EQ.5: rotation about y axis EQ.6: rotation about z axis *CONSTRAINED_SPOTWELD_{OPTION}_{OPTION} If it is desired to use a time filtered force calculation for the forced based failure criterion then the following option is available: <BLANK> FILTERED_FORCE and one additional card must be defined below. To define an ID for the spotweld the following option is available: <BLANK> ID If the ID is defined an additional card is required. The ordering of the options is arbitrary. Purpose: Define massless spot welds between non-contiguous nodal pairs. The spot weld is a rigid beam that connects the nodal points of the nodal pairs; thus, nodal rotations and displacements are coupled. The spot welds must be connected to nodes having rotary inertias, i.e., beams or shells. If this is not the case, for example, if the nodes belong to solid elements, use the option: *CONSTRAINED_RIVET. During implicit calculations this case is treated like a rivet, constraining only the displacements. Note that shell elements do not have rotary stiffness in the normal direction and, therefore, this component cannot be transmitted. Spot welded nodes must not have the same coordinates. Coincident nodes in a spot weld can be handled by the *CONSTRAINED_NODAL_RIGID_BODY option. Brittle and ductile failures are supported by this model. Brittle failure is based on the resultant forces acting on the weld, and ductile failure is based on the average plastic strain value of the shell elements which include the spot welded node. Spot welds, which are connected to massless nodes, are automatically deleted in the initialization phase and a warning message is printed in the messag file and the d3hsp file. Warning. The accelerations of spot welded nodes are output as zero into the various databases, but if the acceleration of spotwelded nodes are required, use either the *CONSTRAINED_GENERALIZED_WELD or the *CONSTRAINED_NODAL_RIGID_- BODY input. However, if the output interval is frequent enough accurate acceleration time histories can be obtained from the velocity time history by differentiation in the post-processing phase. ID Card. Additional card for the ID keyword option. ID 1 2 3 4 5 6 7 8 Variable WID Type Default Card 1 Variable I 0 1 N1 Type I 2 N2 I 3 SN F 4 SS F 5 N F 6 M F 7 TF F 8 EP F Default none none optional optional none none 1.E+20 1.E+20 Remarks 1. 2. 3 4 Filter Card. Additional card for the FILTERED_FORCE keyword option. 3 4 5 6 7 8 Card 2 Variable 1 NF 2 TW Type I F Default none none VARIABLE DESCRIPTION WID Optional weld ID. N1 N2 SN Node ID Node ID Normal force at spotweld failure . VARIABLE DESCRIPTION Shear force at spotweld failure . Exponent for normal spotweld force . Exponent for shear spotweld force . Failure time for nodal constraint set. Effective plastic strain at failure. Number of force vectors stored for filtering. Time window for filtering. SS N M TF EP NF TW Remarks: 1. Nodes connected by a spot weld cannot be members of another constraint set that constrain the same degrees-of-freedom, a tied interface, or a rigid body, i.e., nodes cannot be subjected to multiple, independent, and possibly conflicting constraints. Also, care must be taken to ensure that single point constraints applied to nodes in a constraint set do not conflict with the constraint sets con- strained degrees-of-freedom. 2. Failure of the spot welds occurs when: ) ( ∣𝑓𝑛∣ 𝑆𝑛 + ( ∣𝑓𝑠∣ 𝑆𝑠 ) ≥ 1 where fn and fs are the normal and shear interface force. Component fn is non- zero for tensile values only. 3. When the failure time, TF, is reached the spot weld becomes inactive and the constrained nodes may move freely. 4. Spot weld failure due to plastic straining occurs when the effective nodal plastic 𝑝 . This option can model the tearing out of a strain exceeds the input value,εfail spotweld from the sheet metal since the plasticity is in the material that sur- rounds the spotweld, not the spotweld itself. A least squares algorithm is used to generate the nodal values of plastic strains at the nodes from the element integration point values. The plastic strain is integrated through the element and the average value is projected to the nodes via a least square fit. This op- tion should only be used for the material models related to metallic plasticity and can result is slightly increased run times. Failures can include both the plastic and brittle failures. $$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ $$ $ $$$$ *CONSTRAINED_SPOTWELD $ $$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ $$ $ $ Spotweld two nodes (34574 and 34383) with the approximate strength $ of a 3/8" SAE Grade No 3 bolt. $ *CONSTRAINED_SPOTWELD $ $...>....1....>....2....>....3....>....4....>....5....>....6....>....7....>... .8 $ n1 n2 sn sf n m tf ps 34574 34383 36.0 18.0 2.0 2.0 10. 1.0 $ $ $ sn = 36.0 normal failure force is 36 kN $ sf = 18.0 shear failure force is 18 kN $ n = 2.0 normal failure criteria is raised to the power of 2 $ m = 2.0 shear failure criteria is raised to the power of 2 $ tf = 10.0 failure occurs at time 10 unless strain failure occurs $ ps = 2.0 plastic strain at failure $ $$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ $$ 5. Thermal: The 2 nodes identified by this keyword will be constrained to the same temperature in a thermal problem or in a couple thermal-mechanical problem. *CONSTRAINED Purpose: Define a self-piercing rivet with failure. This model for a self-piercing rivet (SPR2) includes a plastic-like damage model that reduces the force and moment resultants to zero as the rivet fails. The domain of influence is specified by a diameter, which should be approximately equal to the rivet’s diameter. The location of the rivet is defined by a single node at the center of two riveted sheets. The algorithm does a normal projection from the master and slave sheets to the rivet node and locates all nodes within the user-defined diameter of influence. The numerical implementation of this rivet model was developed by L. Olovsson of Impetus Afea, based on research work on SPR point connector models originally carried out by SIMLab (NTNU) and SINTEF, see references by Porcaro, Hanssen, and et.al. [2006, 2006, 2007]. Originally only two sheets (master and slave) could be connected with one SPR2 node. But since release R9, up to 6 sheets can be connected with one SPR2 by defining additional parts on optional card 4. The following stacking sequence should be used: MID – XPID1 – XPID2 – XPID3 – XPID4 – SID. Omitted parts can be left blank, e.g. for a 3-sheet connection the extra part lies in between master and slave, and for a regular 2- sheet connection card 4 can be dropped completely. Card 1 1 2 3 4 Variable MID SID NSID THICK Type I I I F 5 D F 6 FN F 7 FT F 8 DN F Default none none none none none none none none Card 2 Variable 1 DT 2 XIN 3 4 5 6 7 8 XIT ALPHA1 ALPHA2 ALPHA3 DENS INTP Type F F F F F F F F Default none none none none none none none 0.0 *CONSTRAINED_SPR2 Card 3 1 2 3 4 5 6 7 8 Variable EXPN EXPT Type F F Default 8.0 8.0 Card 4 is optional. Card 4 1 2 3 4 5 6 7 8 Variable XPID1 XPID2 XPID3 XPID4 Type I I I I Default none none none none VARIABLE DESCRIPTION MID SID Master sheet Part ID Slave sheet Part ID NSID Node set ID of rivet location nodes. THICK Total thickness of master and slave sheet. D FN FT DN DT XIN XIT Rivet diameter. Rivet strength in tension (pull-out). Rivet strength in pure shear. Failure displacement in normal direction. Failure displacement in tangential direction. Fraction of failure displacement at maximum normal force. Fraction of failure displacement at maximum tangential force. VARIABLE DESCRIPTION ALPHA1 Dimensionless parameter scaling the effective displacement. ALPHA2 Dimensionless parameter scaling the effective displacement. ALPHA3 Dimensionless parameter scaling the effective displacement. The sign of ALPHA3 can be used to choose the normal update procedure: GT.0: incremental update (default), LT.0: total update (recommended). Rivet density (necessary for time step calculation). Flag for interpolation. EQ.0: linear (default), EQ.1: uniform, EQ.2: inverse distance weighting. Exponent value for load function in normal direction. Exponent value for load function in tangential direction. Extra part id 1 for multi-sheet connection. Extra part id 2 for multi-sheet connection. Extra part id 3 for multi-sheet connection. Extra part id 4 for multi-sheet connection. DENS INTP EXPN EXPT XPID1 XPID2 XPID3 XPID4 Self-piercing rivets are a type of fastener that is sometimes used in place of spot welds to join sheet metal of similar or dissimilar materials. The rivet penetrates the first sheet, expands to interlock with the lower sheet without penetration. The strength and fatigue characteristics of self-piercing rivets can meet or even exceed that of spot welds; consequently, their practical applications are expanding. In the local description of the underlying model, all considerations are done in the plane-of-maximum opening defined by The unit normal vectors of the slave and master sheets are 𝐧̂𝑠 and 𝐧̂𝑚 respectively , and tangential unit normal vector of the rivet is 𝐧̂𝑜 = 𝐧̂𝑠 × 𝐧̂𝑚. 𝐧̂𝑡 = 𝐧̂𝑜 × 𝐧̂𝑚. A single-sheet rivet system is assumed, i.e. the rivet translation and rotation follow the motion of the master sheet. The opening appears at the slave sheet. The local deformation is defined by normal stretch vector δ𝑛, tangential stretch 𝛅𝑡 and total stretch δ = δ𝑛 + δ𝑡 . At any given time the total stretch is 𝑠 so that the scalar measures of normal computed from the position vectors: δ = 𝐱𝑠 stretch and tangential stretch are 𝜹𝒏 = δ ⋅ 𝐧̂𝑛 and 𝜹𝒕 = δ ⋅ 𝐧̂𝑡. The normal and tangential forces 𝑓𝑛 and 𝑓𝑡 are then determined by the material model, which will be explained next. 𝑟 − 𝐱𝑠 The moments on the rivet always satisfy, 𝑀𝑚 + 𝑀𝑠 = (ℎ1 + ℎ2)𝑓𝑡/2. The motion, the forces and moments are then distributed to the nodes within the radius of influence by a weighting function, which is, by default, linear . Master Sheet (offset centerline) Slave Sheet Figure 10-39. Plane of maximim opening. Master sheet centerline Rivet Slave sheet centerline Figure 10-40. Single-sheet rivet system. Master sheet Slave sheet Figure 10-41. Local kinematics. Master sheet Slave sheet Figure 10-42. Local forces/moments. The force-deformation relationship is defined by a non-linear damage model for arbitrary mixed-mode loading conditions (combination of tension and shear). For pure tensile and pure shear loading, the behavior is given by, max𝛿𝑡 max𝛿𝑛 𝑓𝑡 𝑓𝑛 fail fail 𝜂max𝛿𝑛 𝜂max𝛿𝑡 𝑓 ̂ 𝑛(𝜂max), 𝑓 ̂ 𝑡(𝜂max) 𝑓𝑛 = 𝑓𝑡 = (1) Respectively where, 𝑓 ̂ 𝑛(𝜂max) = ⎧ {{{ ⎨ {{{ ⎩ 1 − ( 𝜉𝑛 − 𝜂max 𝜉𝑛 EXPN ) 1 − 𝜂max − 𝜉𝑛 1 − 𝜉𝑛 𝑓 ̂ 𝑡(𝜂max) = ⎧ {{{ ⎨ {{{ ⎩ 1 − ( 𝜉𝑡 − 𝜂max 𝜉𝑡 EXPT ) 1 − 𝜂max − 𝜉𝑡 1 − 𝜉𝑡 𝜂max ≤ 𝜉𝑛 𝜂𝑚𝑎𝑥 > 𝜉𝑛 𝜂max ≤ 𝜉𝑡 𝜂𝑚𝑎𝑥 > 𝜉𝑡 (2) In pure tension and pure shear the damage measure, 𝜂max(𝑡), defined in (3), simplifies to coincide with strain as indicated in figure 10-43. Unloading reloading path Unloading reloading path Pure Tension Pure Shear Figure 10-43. Force response of self penetrating rivet. fail can be determined directly max, 𝛿𝑛 Usually, the material parameters 𝑓𝑛 from experiments, whereas material parameters 𝜉𝑛, and 𝜉𝑡 can be found by reverse engineering. For mixed-mode behavior, an effective displacement measure, 𝜂(𝜃), is given by fail, and 𝛿𝑡 max, 𝑓𝑡 𝜂(𝜃, 𝜂max, 𝑡 ) = [𝜉 (𝜃) + 1 − 𝜉 (𝜃) 𝛼(𝜂max) ] √ √√ ⎷ ] [ 𝛿𝑛(𝑡) fail 𝛿𝑛 + [ ] , 𝛿𝑡(𝑡) fail 𝛿𝑡 (3) where, 𝜃 = arctan ( 𝛿𝑛 𝛿𝑡 ) 𝜂max(𝑡) = max[𝜂(𝑡)]. The parameter 𝜉 (𝜃) which ranges from 0 to 1 scales the effective displacement as a function of the direction of the displacement vector in the 𝛿𝑛-𝛿𝑡-plane according to, 𝜉 (𝜃) = 1 − 27 ( 2𝜃 ) + 27 ( 2𝜃 ) . (4) The directional scaling of the effective displacement is allowed to change as damage develops, which is characterized by the shape coefficient 𝛼(𝜂max) defined as 𝛼(𝜂max) = ⎧𝜉𝑡 − 𝜂max { { 𝜉𝑡 ⎨ 1 − 𝜂max { { 1 − 𝜉𝑡 ⎩ 𝛼1 + 𝜂max 𝜉𝑡 𝛼2 𝛼2 + 𝜂max − 𝜉𝑡 1 − 𝜉𝑡 𝜂max < 𝜉𝑡 , 𝛼3 𝜂max ≥ 𝜉𝑡 (5) where 𝛼1, 𝛼2, and 𝛼3 are material parameters. Pull-out Peeling Isolines of (Failure isoline) u e l o a d i n b li q Shear loading Early yielding Figure 10-44. Isosurfaces of 𝜂(𝜃) The directional dependency of the effective displacement is necessary for an accurate force-displacement response in different loading directions. The coefficients 𝛼1, and 𝛼2 decrease the forces in the peeling and oblique loading cases to the correct levels. Both parameters are usually less than 1; whereas 𝛼3 is typically larger than 1 as its main purpose is to moderate the failure displacement in oblique loading directions. Several qualitative features captured by this model are illustrated in Figure 10-44. For the moment distribution, the difference between master sheet (stronger side where the rivet is entered) and slave sheet (weaker side) is accounted for by a gradual transfer from the slave to the master side as damage grows: 𝑀𝑚 = ℎ1 + ℎ2 (1 + 𝜂max − 𝜉1 1 − 𝜉1 ) 𝑓1, 𝑀𝑠 = ℎ1 + ℎ2 (1 − 𝜂max − 𝜉1 1 − 𝜉 ) 𝑓1 (6) Eventually the connection to the slave sheet becomes a moment free hinge. It is recommended to use the drilling rotation constraint method for the connected components in explicit analysis, i.e. parameter DRCPSID of *CONTROL_SHELL should refer to all shell parts involved in SPR2 connections. *CONSTRAINED_TIE-BREAK Purpose: Define a tied shell edge to shell edge interface that can release locally as a function of plastic strain of the shells surrounding the interface nodes. A rather ductile failure is achieved. Card 1 1 2 3 4 5 6 7 8 Variable SNSID MNSID EPPF Type I I F Default none none 0. Remarks 1, 2 3, 4 VARIABLE DESCRIPTION SNSID Slave node set ID, see *SET_NODE_OPTION. MNSID Master node set ID, see *SET_NODE_OPTION. EPPF Plastic strain at failure Remarks: 1. Nodes in the master node set must be given in the order they appear as one moves along the edge of the surface. 2. Tie-breaks may not cross. 3. Tie-breaks may be used to tie shell edges together with a failure criterion on the joint. If the average volume-weighted effective plastic strain in the shell ele- ments adjacent to a node exceeds the specified plastic strain at failure, the node is released. The default plastic strain at failure is defined for the entire tie-break but can be overridden in the slave node set to define a unique failure plastic strain for each node. 4. Tie-breaks may be used to simulate the effect of failure along a predetermined line, such as a seam or structural joint. When the failure criterion is reached in the adjoining elements, nodes along the slideline will begin to separate. As this effect propagates, the tie-breaks will appear to “unzip,” thus simulating failure of the connection. *CONSTRAINED_TIED_NODES_FAILURE Purpose: Define a tied node set with failure based on plastic strain. The nodes must be coincident. Card 1 1 2 3 4 5 6 7 8 Variable NSID EPPF ETYPE Type I F Default none 0. I 0 Remarks 1, 2, 3, 4 VARIABLE DESCRIPTION NSID EPPF Nodal set ID, see *SET_NODE_OPTION. Plastic strain, volumetric strain, or damage (MAT_224) at failure. ETYPE Element type for nodal group: EQ.0: shell, EQ.1: solid element Remarks: 1. This feature applies to solid and shell elements using plasticity material models, and to solid elements using the honeycomb material *MAT_HONEYCOMB (EPPF = plastic volume strain). The failure variable is the volume strain for materials 26, 126, and 201. The failure variable is the damage for material 224, and the equivalent plastic strain is used for all other plasticity models. The specified nodes are tied together until the average volume weighted value of the failure variable exceeds the specified value. Entire regions of individual shell elements may be tied together unlike the tie-breaking shell slidelines. The tied nodes are coincident until failure. When the volume weighted average of the failure value is reached for a group of constrained nodes, the nodes of the elements that exceed the failure value are released to simulate the formation of a crack. 2. To use this feature to simulate failure, each shell element in the failure region should be generated with unique node numbers that are coincident in space with those of adjacent elements. Rather than merging these coincident nodes, the *CONSTRAINED_TIED_NODES_FAILURE option ties the nodal points together. As plastic strain develops and exceeds the failure strain, cracks will form and propagate through the mesh. 3. Entire regions of individual shell elements may be tied together, unlike the *CONSTRAINED_TIE-BREAK option. This latter option is recommended when the location of failure is known, e.g., as in the plastic covers which hide airbags in automotive structures. 4. When using surfaces of shell elements defined using the *CONSTRAINED_- TIED_NODES_FAILURE option in contact, it is best to defined each node in the surface as a slave node with the NODE_TO_SURFACE contact options. If this is not possible, the automatic contact algorithms beginning with *CONTACT_- AUTOMATIC_... all of which include thickness offsets are recommended. Example: $$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ $ $$$$ *CONSTRAINED_TIED_NODES_FAILURE $ $$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ $ $ Tie shell elements together at the nodes specified in nodal set 101. The $ constraint will be broken when the plastic strain at the nodes exceeds 0.085. $ $ In this example, four shell elements come together at a common point. $ The four corners of the shells are tied together with failure as opposed $ to the more common method of merging the nodes in the pre-processing stage. $ *CONSTRAINED_TIED_NODES_FAILURE $ $...>....1....>....2....>....3....>....4....>....5....>....6....>....7....>....8 $ nsid eppf 101 0.085 $ $ *SET_NODE_LIST $ sid 101 $ nid1 nid2 nid3 nid4 nid5 nid6 nid7 nid8 775 778 896 897 $ $$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ The keyword *CONTACT provides a way of treating interaction between disjoint parts. Different types of contact may be defined: *CONTACT_OPTION1_{OPTION2}_{OPTION3}_{OPTION4}_{OPTION5} *CONTACT_ADD_WEAR *CONTACT_AUTO_MOVE *CONTACT_COUPLING *CONTACT_ENTITY *CONTACT_GEBOD_OPTION *CONTACT_GUIDED_CABLE *CONTACT_INTERIOR *CONTACT_RIGID_SURFACE *CONTACT_1D *CONTACT_2D_OPTION1_{OPTION2}_{OPTION3} The first, *CONTACT_..., is the general 3D contact algorithms. The second, *CON- TACT_COUPLING, provides a means of coupling to deformable surfaces to MADY- MO. The third, *CONTACT_ENTITY, treats contact using mathematical functions to describe the surface geometry for the master surface. The fourth, *CONTACT_GEBOD is a specialized form of the contact entity for use with the rigid body dummies . The fifth, *CONTACT_INTERIOR, is under development and is used with soft foams where element inversion is sometimes a problem. Contact between layers of brick elements is treated to eliminate negative volumes. The sixth, *CONTACT_RIGID_SURFACE is for modeling road surfaces for durability and NVH calculations. The seventh, *CONTACT_1D, remains in LS-DYNA for historical reasons, and is sometimes still used to model rebars which run along edges of brick elements. The last, *CONTACT_2D, is the general 2D contact algorithm based on those used previously in LS-DYNA2D. *CONTACT_OPTION1_{OPTION2}_{OPTION3}_{OPTION4}_{OPTION5}_{OPTION6} Purpose: Define a contact interface in a 3D model. For contact in 2D models, see *CONTACT_2D_OPTION. OPTIONS FOR *CONTACT KEYWORD OPTION REQUIRED DESCRIPTION OPTION1 OPTION2 OPTION3 OPTION4 OPTION5 OPTION6 Yes Specifies contact type No No No No No Flag for thermal Flag indicating ID cards follow Offset options Flag for MPP Flag for orthotropic friction Allowed values for OPTION1 All contact types are available for explicit and implicit calculations. AIRBAG_SINGLE_SURFACE AUTOMATIC_BEAMS_TO_SURFACE AUTOMATIC_GENERAL AUTOMATIC_GENERAL_EDGEONLY AUTOMATIC_GENERAL_INTERIOR AUTOMATIC_NODES_TO_SURFACE AUTOMATIC_NODES_TO_SURFACE_SMOOTH AUTOMATIC_ONE_WAY_SURFACE_TO_SURFACE AUTOMATIC_ONE_WAY_SURFACE_TO_SURFACE_TIEBREAK AUTOMATIC_ONE_WAY_SURFACE_TO_SURFACE_SMOOTH AUTOMATIC_SINGLE_SURFACE AUTOMATIC_SINGLE_SURFACE_MORTAR AUTOMATIC_SINGLE_SURFACE_SMOOTH AUTOMATIC_SINGLE_SURFACE_TIED AUTOMATIC_SURFACE_TO_SURFACE AUTOMATIC_SURFACE_TO_SURFACE_MORTAR AUTOMATIC_SURFACE_TO_SURFACE_MORTAR_TIED AUTOMATIC_SURFACE_TO_SURFACE_TIED_WELD AUTOMATIC_SURFACE_TO_SURFACE_TIEBREAK AUTOMATIC_SURFACE_TO_SURFACE_TIEBREAK_MORTAR AUTOMATIC_SURFACE_TO_SURFACE_SMOOTH CONSTRAINT_NODES_TO_SURFACE CONSTRAINT_SURFACE_TO_SURFACE DRAWBEAD ERODING_NODES_TO_SURFACE ERODING_SINGLE_SURFACE ERODING_SURFACE_TO_SURFACE FORCE_TRANSDUCER_CONSTRAINT FORCE_TRANSDUCER_PENALTY FORMING_NODES_TO_SURFACE FORMING_NODES_TO_SURFACE_SMOOTH FORMING_ONE_WAY_SURFACE_TO_SURFACE FORMING_SURFACE_TO_SURFACE_MORTAR FORMING_ONE_WAY_SURFACE_TO_SURFACE_SMOOTH FORMING_SURFACE_TO_SURFACE FORMING_SURFACE_TO_SURFACE_SMOOTH NODES_TO_SURFACE NODES_TO_SURFACE_INTERFERENCE NODES_TO_SURFACE_SMOOTH ONE_WAY_SURFACE_TO_SURFACE ONE_WAY_SURFACE_TO_SURFACE_INTERFERENCE ONE_WAY_SURFACE_TO_SURFACE_SMOOTH RIGID_NODES_TO_RIGID_BODY RIGID_BODY_ONE_WAY_TO_RIGID_BODY RIGID_BODY_TWO_WAY_TO_RIGID_BODY SINGLE_EDGE SINGLE_SURFACE SLIDING_ONLY SLIDING_ONLY_PENALTY SPOTWELD SPOTWELD_WITH_TORSION SPOTWELD_WITH_TORSION_PENALTY SURFACE_TO_SURFACE SURFACE_TO_SURFACE_INTERFERENCE SURFACE_TO_SURFACE_SMOOTH SURFACE_TO_SURFACE_CONTRACTION_JOINT TIEBREAK_NODES_TO_SURFACE TIEBREAK_NODES_ONLY TIEBREAK_SURFACE_TO_SURFACE TIED_NODES_TO_SURFACE TIED_SHELL_EDGE_TO_SURFACE TIED_SHELL_EDGE_TO_SOLID TIED_SURFACE_TO_SURFACE TIED_SURFACE_TO_SURFACE_FAILURE Allowed values for OPTION2: THERMAL THERMAL_FRICTION NOTE: THERMAL and THERMAL_FRICTION options are restricted to contact types having “SURFACE_TO_- SURFACE” in OPTION1. Allowed value for OPTION3: ID Allowed values for OPTION4: OPTION4 specifies that offsets may be used with the tied contact types. If one of these three offset options is set, then offsets are permitted for these contact types, and, if not, the nodes are projected back to the contact surface during the initialization phase and a constraint formulation is used. Note that in a constraint formulation, the nodes of rigid bodies are not permitted in the definition. OFFSET The OFFSET option switches the formulation from a constraint type formulation to one that is penalty based where the force and moment (if applicable) result- ants are transferred by discrete spring elements between the slave nodes and master segments. OFFSET is available when OPTION1 is: TIED_NODES_TO_SURFACE TIED_SHELL_EDGE_TO_SURFACE TIED_SURFACE_TO_SURFACE With this option, there is no coupling between the transmitted forces and mo- ments and thus equilibrium is not enforced. In the TIED_SHELL_EDGE_TO_- SURFACE contact, the BEAM_OFFSET option may be preferred since corresponding moments accompany transmitted forces. Rigid bodies can be used with this option. BEAM_OFFSET The BEAM_OFFSET option switches the formulation from a constraint type formulation to one that is penalty based. Beam-like springs are used to transfer force and moment resultants between the slave nodes and the master segments. Rigid bodies can be used with this option. BEAM_OFFSET is available when OPTION1 is: TIED_SHELL_EDGE_TO_SURFACE SPOTWELD CONSTRAINED_OFFSET The CONSTRAINED_OFFSET option is a constraint type formulation. CONSTRAINED_OFFSET is available when OPTION1 is: TIED_NODES_TO_SURFACE TIED_SHELL_EDGE_TO_SURFACE TIED_SURFACE_TO_SURFACE SPOTWELD Allowed value OPTION5: MPP Allowed value for OPTION6: ORTHO_FRICTION Remarks 1. Smooth Contact. For SMOOTH contact, a smooth curve-fitted surface is used to represent the master segment, so that it can provide a more accurate repre- sentation of the actual surface, reduce the contact noise, and produce smoother results with coarser meshes. All contact options that include SMOOTH are available for MPP. Only the FORMING contacts, wherein the master side is rigid, can be used with SMOOTH in the case of SMP. For SURFACE_TO_SURFACE and SINGLE_SURFACE contacts with SMOOTH in MPP, both the slave and master sides are smoothed every cycle, thereby slowing the contact treatment considerably. The SMOOTH option does not apply to segment based (SOFT = 2) contacts. 2. Automatic General Contact. *CONTACT_AUTOMATIC_GENERAL is a single surface contact similar to *CONTACT_AUTOMATIC_SINGLE_SUR- FACE but which includes treatment of beam-to-beam contact and in doing so, checks along the entire length of the beams for penetration. *CONTACT_AU- TOMATIC_GENERAL essentially adds null beams to the exterior edges of shell parts so that edge-to-edge treatment of the shell parts is handled by virtue of contact of the automatically-generated null beams. By adding the word INTE- RIOR to *CONTACT_AUTOMATIC_GENERAL, the contact algorithm goes a step further by adding null beams to all the shell meshlines, both along the exterior, unshared edges and the interior, shared shell edges. The EDGEONLY option skips the node-to-surface contact and does only the edge-to-edge and beam-to-beam contact. 3. Recommendations for TIED Contact Types. For tying solids-to-solids, that is, for situations where none of the nodes have rotational degrees-of-freedom, use TIED_NODES_TO_SURFACE and TIED_SURFACE_TO_SURFACE type contacts. These contact types may include the OFFSET or CONSTRAINED_- OFFSET option. For tying shells-to-shells, beams-to-shells, that is, for situations where all the nodes have rotational degrees-of-freedom, use TIED_SHELL_EDGE_TO_SUR- FACE type contacts. This contact type may include the OFFSET, CON- STRAINED_OFFSET, or BEAM_OFFSET option. TIED_SHELL_EDGE_TO_SOLID is intended for tying shell edges to solids or beam ends to solids, that is, situations where only the slave side nodes have rotational degrees-of-freedom. 4. Tied Contact Types and the Implicit Solver. Non-physical results have been observed when the implicit time integrator is used for models that combine tied contact formulations with automatic single point constraints on solid element rotational degrees of (AUTOSPC on *CONTROL_IMPLICIT_- SOLVER). The following subset of tied interfaces support a strongly objective mode and verified to behave correctly with the implicit time integrator: freedom 1) TIED_NODES_TO_SURFACE_CONSTRAINED_OFFSET 2) TIED_NODES_TO_SURFACE_OFFSET 3) TIED_SHELL_EDGE_TO_SURFACE_CONSTRAINED_OFFSET 4) TIED_SHELL_EDGE_TO_SURFACE_BEAM_OFFSET The first two of these ignore rotational degrees of freedom, while the third and fourth constrain rotations. The first and third are constraint based; while the second and fourth are penalty based. These four contact types are intended to cover most use scenarios. Setting IACC = 1 on *CONTROL_ACCURACY activates the strongly objective formulation for the above mentioned contacts (as well as the non-offset options *CONTACT_TIED_NODES_TO_SURFACE and *CONTACT_TIED_SHELL_- EDGE_TO_SURFACE as a side effect). When active, forces and moments trans- form correctly under superposed rigid body motions within a single implicit step. Additionally, this formulation applies rotational constraints consistently when, and only when, necessary. In particular, strong objectivity is implemented so that slave nodes without rotational degrees of freedom are not rotationally constrained, while slave nodes with bending and torsional rotations are rota- tionally constrained. Additionally, strong objectivity ensures that the constraint is physically correct. For a master node belonging to a shell, the slave node’s bending rotations (rota- tions in the plane of the master segment) are constrained to match the master segment’s rotational degrees of freedom; for master nodes not belonging to a shell, the slave’s bending rotations are constrained to the master segment rota- tion as determined from its individual nodal translations. The slave node’s torsional rotations (rotations with respect to the normal of the master segment) are always constrained based on the master segment’s torsional rotation as de- termined from its individual nodal translations, thus avoiding the relatively weak drilling mode of shells. This tied contact formulation properly treats bending and torsional rotations. Since slave node rotational degrees of freedom typically come from shell or beam elements the most frequently used options are: TIED_SHELL_EDGE_TO_SURFACE_CONSTRAINED_OFFSET TIED_SHELL_EDGE_TO_SURFACE_BEAM_OFFSET The other two “non-rotational” formulations: TIED_NODES_TO_SURFACE_CONSTRAINED_OFFSET TIED_NODES_TO_SURFACE_OFFSET are included for situations in which rotations do not need to be constrained at all. See the LS-DYNA Theory Manual for further details. 5. Additional Remarks. Additional notes on contact types and a few examples are provided at the end of this section in “General Remarks: *CONTACT”. A theoretical discussion is provided in the LS-DYNA Theory Manual. ADDITIONAL CARDS FOR *CONTACT KEYWORD Cards must appear in the exact order listed below. CARD ID MPP Card 1 Card 2 Card 3 Card 4 DESCRIPTION Card required when OPTION3 set to ID option; otherwise this card is omitted. Card required when OPTION5 set to MPP. Always required. Always required. Always required. Required for the following permutations of *CONTACT. NOTE: The format of Card 4 is different for each option listed below. *CONTACT_AUTOMATIC_SINGLE_SURFACE_TIED *CONTACT_CONSTRAINT_type *CONTACT_DRAWBEAD *CONTACT_ERODING_type *CONTACT_…_INTERFERENCE *CONTACT_RIGID_type *CONTACT_TIEBREAK_type *CONTACT_…_CONTRACTION_JOINT_type THERMAL Required if OPTION2 is set. Otherwise omit. THERMAL_FRICTION Required if OPTION2 is set to THERMAL_FRICTION. Otherwise omit. ORTHO_FRICTION Required if OPTION6 is set. Otherwise omit. Contains friction coefficients CARD DESCRIPTION Optional Card A Optional parameters. NOTE: Default values are highly optimized. NOTE: Required if Optional Card B is includ- ed. If Optional Card A is a blank line, then values are set to their defaults, and Optional Card B may follow. Optional Card B Optional parameters. Required if Optional Card C is included. Optional Card C Optional parameters. Required if Optional Card D is included. Optional Card D Optional parameters. Required if Optional Card E is included. Optional Card E Optional parameters. *CONTACT_OPTION1_{OPTION2}_… Additional keyword for ID keyword option. ID 1 2 3 4 5 6 7 8 Variable CID Type I HEADING A70 The contact ID is needed during full deck restarts for contact initialization. If the contact ID is undefined, the default ID is determined by the sequence of the contact definitions, i.e., the first contact definition has an ID of 1, the second, 2, and so forth. In a full deck restart without contact IDs, for a successful run no contact interfaces can be deleted and those which are added must be placed after the last definition in the previous run. The ID and heading is picked up by some of the peripheral LS-DYNA codes to aid in post-processing. VARIABLE DESCRIPTION CID Contact interface ID. This must be a unique number. HEADING Interface descriptor. It is suggested that unique descriptions be used. MPP Cards. Variables set with these cards are only active when using MPP LS- DYNA. MPP Card 1. Additional card for the MPP option. This card is ignored, but still read in, when SOFT = 2 on optional card A. MPP 1 1 2 3 4 5 6 7 8 Variable IGNORE BCKT LCBCKT NS2TRK INITITR PARMAX CPARM8 Type I I I Default 0 200 none I 3 I 2 F See below I 0 MPP Card 2. The keyword reader will interpret the card following MPP Card 1 as MPP Card 2 if the first column of the card is occupied by an ampersand. Otherwise, it is interpreted as Card 1. This card is ignored, but still read in, when SOFT = 2 on optional card A. MPP 2 Variable 1 & 2 3 4 5 6 7 8 CHKSEGS PENSF GRPABLE Type Default I 0 F 1.0 I IGNORE BCKT LCBCKT NS2TRK INITITR PARMAX *CONTACT_OPTION1_{OPTION2}_… DESCRIPTION This is the same as the “ignore initial penetrations” option on the *CONTROL_CONTACT Optional Card C entry 2 and can also be specified in the normal contact control cards. It predates both of those, and is not really needed anymore since both are honored by the MPP code. That is, if any of the three are on, initial penetrations are tracked. Bucket sort frequency, this parameter does not apply when SOFT = 2 on optional card A or to the Mortar contact (option MORTAR on the CONTACT card). For the two exceptions, the BSORT option on Optional Card A applies instead. Load curve for bucket sort frequency, this parameter does not apply when SOFT = 2 on optional card A or to the Mortar contact (option MORTAR on the CONTACT card). For the two exceptions, the negative BSORT option on Optional Card A applies instead. Number of potential contacts to track for each slave node. The normal input for this (DEPTH on Optional Card A) is ignored. Number of iterations to perform when trying to eliminate initial penetrations. Note: an input of 0 means 0, not the default value (which is 2). Leaving this field blank will set INITITR to 2. The parametric extension distance for contact segments. The MAXPAR parameter on Optional Card A is not used for MPP. For non-TIED contacts, the default is 1.0005. For TIED contacts the default is 1.035 and, the actual extension used is computed as follows: PARMAXcomputed= ⎧1.0 + PARMAX {{ ⎨ {{ ⎩ PARMAX max(PARMAX, 1.035) 0.0 < PARMAX < 0.5 1.0 ≤ PARMAX ≤ 1.0004 otherwise VARIABLE CPARM8 CHKSEGS PENSF DESCRIPTION Flag for CONTACT_AUTOMATIC_GENERAL behavior. CPAR- M8’s value is interpreted as two separate flags: OPT1 and OPT2 according to the rule, CPARM8 = OPT1 + OPT2. When OPT1 and OPT2 are both set, both options are active. OPT1: Flag to exclude beam-to-beam contact from the same PID. EQ.0: Flag is not set (default). EQ.1: Flag is set. EQ.2: Flag is set. CPARM8 = 2 has the additional effect of permitting contact treatment of spot weld (type 9) beams in AUTOMATIC_GENERAL contacts; spot weld beams are otherwise disregarded entirely by AU- TOMATIC_GENERAL contacts. OPT2: Flag to shift generated beam affecting only shell-edge-to- shell-edge treatment. See also SRNDE in Optional Card E. EQ.10: Beam generated on exterior shell edge will be shifted into the shell by half the shell thickness. Therefore, the shell-edge-to-shell-edge contact starts right at the shell edge and not at an extension of the shell edge. If this value is non-zero, then the node to surface and surface to surface contacts will perform a special check at time 0 for elements that are inverted (or nearly so), and remove them from contact. These poorly formed elements have been known to occur on the tooling in metalforming problems, which allows these problems to run. It should not normally be needed for reasonable meshes. This option is used together with IGNORE for 3D forging problems. If non-zero, the IGNORED penetration distance is multiplied by this value each cycle, effectively pushing the slave node back out to the surface. This is useful for nodes that might get generated below the master surface during 3D remeshing. Care should be exercised, as energy may be generated and stability may be effected for values lower than 0.95. A value in the range of 0.98 to 0.99 or higher (but < 1.0) is recommended. GRPABLE *CONTACT_OPTION1_{OPTION2}_… DESCRIPTION Set to 1 to invoke an alternate MPP communication algorithm for SINGLE_SURFACE, NODE_TO_SURFACE, and SURFACE_TO_- SURFACE contacts. The new algorithm does not support all contact options, including SOFT = 2, as of yet, and is still under development. It can be significantly faster and scale better than the normal algorithm when there are more than two or three applicable contact types defined in the model. Its intent is to speed up the contact processing but not to change the behavior of *CONTROL_MPP_CONTACT_- contact. the GROUPABLE. also See Remarks: 1. The MPP cards are ignored by the segment based contact options that are made active by setting SOFT = 2 on optional card A. When SOFT = 2. The BSORT parameter on optional card A can be used to override the default bucket sort frequency. Card 1. Card 1 1 2 3 4 5 6 7 8 Variable SSID MSID SSTYP MSTYP SBOXID MBOXID SPR MPR Type I I I I I I Default none none none none I 0 I 0 Remarks 1 2 optional optional 0 = off 0 = off VARIABLE SSID DESCRIPTION Slave segment, node set ID, part set ID, part ID, or shell element set ID, see *SET_SEGMENT, *SET_NODE_OPTION, *PART, *SET_PART or *SET_SHELL_OPTION. For ERODING_SINGLE_- SURFACE and ERODING_SURFACE_TO_SURFACE contact types, use either a part ID or a part set ID. For ERODING_- NODES_TO_SURFACE contact, use a node set which includes all nodes that may be exposed to contact as element erosion occurs. EQ.0: all part IDs are included for single surface contact, automatic single surface, and eroding single surface. MSID Master segment set ID, part set ID, part ID, or shell element set ID, see *SET_SEGMENT, *SET_NODE_OPTION, *PART, *SET_- PART, or *SET_SHELL_OPTION: EQ.0: for single surface contact, automatic single surface, and eroding single surface. VARIABLE DESCRIPTION SSTYP ID type of SSID: EQ.0: segment set ID for surface-to-surface contact, EQ.1: shell element set ID for surface-to-surface contact, EQ.2: part set ID, EQ.3: part ID, EQ.4: node set ID for node to surface contact, EQ.5: include all (SSID is ignored), EQ.6: part set ID for exempted parts. All non-exempted parts are included in the contact. For *AUTOMATIC_BEAMS_TO_SURFACE contact either a part set ID or a part ID can be specified. MSTYP ID type of MSID: EQ.0: segment set ID, EQ.1: shell element set ID, EQ.2: part set ID, EQ.3: part ID. SBOXID MBOXID EQ.4: node set ID (for eroding force transducer only. See remark 3), EQ.5: include all (MSID is ignored). Include in contact definition only those slave nodes/segments within box SBOXID (corresponding to BOXID in *DEFINE_BOX), or if SBOXID is negative, only those slave nodes/segments within contact volume |SBOXID| (corresponding to CVID in *DEFINE_CONTACT_VOLUME). SBOXID can be used only if SSTYP is set to 2 or 3, i.e., SSID is a part ID or part set ID. SBOX- ID is not available for_ERODING contact options. Include in contact definition only those master segments within box MBOXID (corresponding to BOXID in *DEFINE_BOX), or if MBOXID is negative, only those master segments within contact volume |MBOXID| (corresponding to CVID in *DEFINE_CON- TACT_VOLUME). MBOXID can be used only if MSTYP is set to 2 or 3, i.e., MSID is a part ID or part set ID. MBOXID is not available for_ERODING contact options DESCRIPTION Include the slave side in the *DATABASE_NCFORC and the *DATABASE_BINARY_INTFOR files, and optionally in the dynain file for wear: interface force EQ.1: slave side forces included. EQ.2: same as EQ.1, but also allows for slave nodes to be written as *INITIAL_CONTACT_WEAR to dynain, see NCYC on *INTERFACE_SPRINGBACK_LSDYNA. Include the master side in the *DATABASE_NCFORC and the *DATABASE_BINARY_INTFOR files, and optionally in the dynain file for wear: interface force EQ.1: master side forces included. EQ.2: same as EQ.1, but also allows for master nodes to be written as *INITIAL_CONTACT_WEAR to dynain, see NCYC on *INTERFACE_SPRINGBACK_LSDYNA. VARIABLE SPR MPR Remarks: 1. Giving a slave set ID equal to zero is valid only for the single surface contact algorithms, i.e., the options: SINGLE_SURFACE AUTOMATIC_… AIRBAG_… ERODING_SINGLE_SURFACE 2. A master set ID is not defined for the single surface contact algorithms (including AUTOMATIC_GENERAL). A master set ID is optional for FORCE_- TRANSDUCERS. If a master set is defined for the FORCE_TRANSDUCER option, only those force that develop between and master and slave surfaces are considered. If a transducer is used for extracting forces from Mortar contacts, the slave and master sides must be defined through parts or part sets, segment or node sets will not gather the correct data. NOTE: The master surface option of FORCE_TRANSDUC- ER is only implemented for the PENALTY option and works only in conjunction with the AUTO- MATIC_SINGLE_SURFACE contact types, except as noted in the next remark. 3. A master node set can only be used with the TRANSDUCER_PENALTY option, and requires that the slave side also be defined via a node set. This allows the transducer to give correct results for eroding materials. The node sets should include all nodes that may be exposed as erosion occurs. This option does not apply to Mortar contacts. Card 2. Card 2 Variable 1 FS Type F Default 0. Remarks 2 FD F 0. 3 DC F 0. 4 VC F 0. 5 6 7 VDC PENCHK BT 8 DT F F F 0. I 0 0. 1.0E20 VARIABLE DESCRIPTION If OPTION1 is TIED_SURFACE_TO_SURFACE_FAILURE, then FS Normal tensile stress at failure. failure occurs if [ max(0.0, 𝜎normal) ] 𝐹𝑆 + [ 𝜎shear 𝐹𝐷 ] > 1 where 𝜎normal and 𝜎shear are the interface normal and shear stresses. FD Shear stress at failure. See FS. Else 𝜇 𝑝3 𝑝2 𝑝1 𝑣re Figure 11-1. Friction coefficient, 𝜇, can be a function of relative velocity and pressure. See Remarks for FS = 2.0. VARIABLE DESCRIPTION FS Static coefficient of friction. If FS is > 0 and not equal to 2. The frictional coefficient is assumed to be dependent on the relative velocity 𝑣rel of the surfaces in contact according to, 𝜇𝑐 = FD + (FS − FD)𝑒−DC∣𝑣rel∣. For mortar contact 𝜇𝑐 = FS, i.e., dynamic effects are ignored. The two other possibilities are: EQ.-2: If only the one friction table is defined using *DEFINE_- FRICTION, it will be used and there is no need to de- fine parameter FD. If more than one friction table is defined then the Table ID is defined by the FD Parame- ter below. EQ.-1: If the frictional coefficients defined in the *PART section are to be used, set FS to the negative number, -1.0. WARNING: Please note that the FS = -1.0 and FS = -2.0 options apply only to contact types: SINGLE_SURFACE, AUTOMATIC_GENERAL, AUTOMATIC_SINGLE_SURFACE, AUTOMATIC_SINGLE_SURFACE_MORTAR, AUTOMATIC_NODES_TO_SURFACE, VARIABLE DESCRIPTION AUTOMATIC_SURFACE_TO_SURFACE, AUTOMATIC_SURFACE_TO_SURFACE_MORTAR, AUTOMATIC_ONE_WAY_SURFACE_TO_SURFACE, ERODING_SINGLE_SURFACE. EQ.2: For a subset of SURFACE_TO_SURFACE type contacts , the variable FD serves as a table ID . That table speci- fies two or more values of contact pressure, with each pressure value in the table corresponding to a curve of friction coefficient vs. relative velocity. Thus the fric- tion coefficient becomes a function of pressure and rela- tive velocity. See Figure 11-1. FD Dynamic coefficient of friction. The frictional coefficient is assumed to be dependent on the relative velocity 𝑣rel of the surfaces in contact according to, 𝜇𝑐 = FD + (FS − FD)𝑒−𝐷𝐶∣𝑣rel∣ For mortar contact 𝜇𝑐 = FS, i.e., dynamic effects are ignored. When FS = -2: If FS = -2 and more than one friction table is defined, FD is used to specify friction table to be used. End If DC VC The frictional coefficient is Exponential decay coefficient. assumed to be dependent on the relative velocity 𝑣rel of the surfaces in contact 𝜇𝑐 = FD + (FS − FD)𝑒−DC∣vrel∣. For mortar contact 𝜇𝑐 = FS, i.e., dynamic effects are ignored. Coefficient for viscous friction. This is necessary to limit the friction force to a maximum. A limiting force is computed 𝐹lim = VC × 𝐴cont. 𝐴cont being the area of the segment contacted by the node in contact. The suggested value for VC is the yield where 𝜎0 is the yield stress of the stress in shear 𝑉𝐶 = 𝜎𝑜 √3 contacted material. VDC *CONTACT_OPTION1_{OPTION2}_… DESCRIPTION Viscous damping coefficient in percent of critical or the coefficient of restitution expressed as percentage. In order to avoid in contact, e.g., for sheet forming undesirable oscillation simulation, a contact damping perpendicular to the contacting surfaces is applied. When ICOR, the 6th column of the optional E card, is not defined or 0, the applied damping coefficient is given by 𝜉 = VDC 100 𝜉crit, where VDC is an integer (in units of percent) between 0 and 100. The formula for critical damping is 𝜉crit = 2𝑚𝜔, where 𝑚 is determined by nodal masses as 𝑚 = min(𝑚slave, 𝑚master), and 𝜔 is determined from 𝑘, the interface stiffness, according to 𝜔 = √𝑘 𝑚slave + 𝑚master 𝑚master𝑚slave . PENCHK Small penetration in contact search option. If the slave node penetrates more than the segment thickness times the factor XPENE, see *CONTROL_CONTACT, the penetration is ignored and the slave node is set free. The thickness is taken as the shell thickness if the segment belongs to a shell element or it is taken as 1/20 of its shortest diagonal if the segment belongs to a solid element. This option applies to the surface-to-surface contact algorithms: See Table 11-17 for contact types and more details. BT Birth time (contact surface becomes active at this time). LT.0: Birth time is set to |BT|. When negative, birth time is followed during the dynamic relaxation phase of the calculation. After dynamic relaxation has completed, contact is activated regardless the value of BT. EQ.0: Birth time is inactive, i.e., contact is always active GT.0: If DT = -9999, BT is interpreted as the curve or table ID defining multiple pairs of birth-time/death-time, see remarks below. Otherwise, if DT > 0, birth time applies both during and after dynamic relaxation. DT Death time (contact surface is deactivated at this time). VARIABLE DESCRIPTION LT.0: If DT = -9999, BT is interpreted as the curve or table ID defining multiple pairs of birth-time/death-time. Oth- erwise, negative DT indicates that contact is inactive during dynamic relaxation. After dynamic relaxation the birth and death times are followed and set to |BT| and |DT| respectively. EQ.0: DT defaults to 1.E+20. GT.0: DT, the death time, sets the time at which the contact is deactivated. Remarks: The FS = 2 method of specifying the friction coefficient as a function of pressure and relative velocity is implemented in all contacts for which SOFT = 2. It is recommended that when FS = 2 and SOFT = 2 are used together, that FNLSCL be set in the range of 0.5 to 1.0 and DNLSCL be set to 0 (refer to Remark 5 under the description of Optional Card D for *CONTACT). If sliding is prevalent, DPRFAC = 0.01 on Optional Card C is also recommended. When FS = 2 and SOFT = 0 or 1, the following ONE_WAY contacts are recommended. If sliding is prevalent, DPRFAC = 0.01 is also recommended. ONE_WAY_SURFACE_TO_SURFACE (SMP and MPP) AUTOMATIC_ONE_WAY_SURFACE_TO_SURFACE (MPP only) FORMING_ONE_WAY_SURFACE_SURFACE_TO_SURFACE (MPP only) For SOFT = 0 or 1, FS = 2 is implemented but not advised for the following contacts: SURFACE_TO_SURFACE AUTOMATIC_SURFACE_TO_SURFACE FORMING_SURFACE_TO_SURFACE (SMP and MPP) (MPP only) (MPP only) A caveat pertaining to the MPP contacts listed above is that the “groupable” option must not be invoked. See *CONTROL_MPP_CONTACT_GROUPABLE. For SOFT = 0 or 1, FS = 2 is not implemented in SMP for AUTOMATIC and FORMING contact types. The static friction coefficient will literally be taken as 2.0 if FS is set to 2 for these SMP contacts. If DT = -9999, BT is taken to be the ID of an activation curve defining multiple birth- times and death-times as ordered (𝑥, 𝑦) pairs. A data point in the activation curve defines a time slot during which the contact is active. For example, an activation curve with two data points of (20, 30) and (50, 70) activates the contact when 20 ≤ time ≤ 30 and when 50 ≤ time ≤ 70. To define separate activation curves for dynamic relaxation and the subsequent dynamics, BT can be defined as a table containing two activation curves, one with VALUE = 0 for transient analysis and the other one with VALUE = 1 for dynamic relaxation, see *DEFINE_TABLE. Card 3. Card 3 1 2 3 4 5 6 7 8 Variable SFS SFM SST MST SFST SFMT FSF VSF Type F F F F F F F F Default 1. 1. element thickness element thickness 1. 1. 1. 1. VARIABLE DESCRIPTION SFS SFM SST MST SFST Scale factor on default slave penalty stiffness when SOFT = 0 or SOFT = 2, see also *CONTROL_CONTACT. Scale factor on default master penalty stiffness when SOFT = 0 or SOFT = 2, see also *CONTROL_CONTACT. Optional contact thickness for slave surface (overrides default contact thickness). This option applies to contact with shell and beam elements. SST has no bearing on the actual thickness of the elements; it only affects the location of the contact surface. For the *CONTACT_TIED_… options, SST and MST below can be defined as negative values, which will cause the determination of whether or not a node is tied to depend only on the separation distance relative to the absolute value of these thicknesses. More information is given under General Remarks on *CONTACT following Optional Card E. Optional contact thickness for master surface (overrides default contact thickness). This option applies only to contact with shell elements. For the TIED options, see SST above. Scale factor applied to contact thickness of slave surface. This option applies to contact with shell and beam elements. SFST has no bearing on the actual thickness of the elements; it only affects the location of the contact surface. SFST is ignored if SST is nonzero except in the case of MORTAR contact . SFMT FSF VSF Remarks: *CONTACT_OPTION1_{OPTION2}_… DESCRIPTION Scale factor applied to contact thickness of master surface. This option applies only to contact with shell elements. SFMT has no bearing on the actual thickness of the elements; it only affects the location of the contact surface. SFMT is ignored if MST is nonzero except in the case of MORTAR contact . Coulomb friction scale factor. The Coulomb friction value is scaled as 𝜇𝑠𝑐 = FSF × 𝜇𝑐, see above. Viscous friction scale factor. If this factor is defined then the limiting force becomes: 𝐹lim = VSF × VC × 𝐴cont, see above. The variables FSF and VSF above can be overridden segment by segment on the *SET_- SEGMENT or *SET_SHELL_OPTION cards for the slave surface only as A3 and A4, and for the master surface only as A1 and A2. See *SET_SEGMENT and *SET_SHELL_ OPTION. Card 4: AUTOMATIC_SURFACE_TIEBREAK This card 4 is mandatory for: *CONTACT_AUTOMATIC_SURFACE_TO_SURFACE_TIEBREAK_{OPTION} *CONTACT_AUTOMATIC_ONE_WAY_SURFACE_TO_SURFACE_TIEBREAK_{OPTION} If the response parameter OPTION below is set to 9 or 11, three damping constants can be defined for the various failure modes. To do this, set the keyword option to DAMPING For OPTION = 7 and OPTION = 9 but for the automatic surface to surface contact only, the mortar treatment of the tiebreak contact may be activated. This is primarily intended for implicit analysis and no damping can be used with this option, see also remarks on mortar contacts. The keyword option for this is MORTAR The mortar treatment of tiebreak contact is available only for OPTION = 7 and OP- TION = 9, and only with surface to surface contact, i.e., neither the ONE_WAY nor the DAMPING option is compatible with the MORTAR option. Card 4a 1 2 3 4 5 6 7 8 Variable OPTION NFLS SFLS PARAM ERATEN ERATES CT2CN CN Type I F F F F F F F Default required required required 0.0 0.0 0.0 1.0 0.0 Damping Card. Additional card for the case of OPTION = 9 with the DAMPING keyword option active. Card 4b 1 2 3 4 5 6 7 8 Variable DMP_1 DMP_2 DMP_3 Type F F F Default 0.0 0.0 0.0 VARIABLE DESCRIPTION OPTION Response: EQ.-3: see 3, moments are transferred. SMP only. EQ.-2: see 2, moments are transferred. SMP only. EQ.-1: see 1, moments are transferred. SMP only. EQ.1: slave nodes in contact and which come into contact will permanently stick. Tangential motion is inhibited. EQ.2: tiebreak is active for nodes which are initially in contact. Until failure, tangential motion is inhibited. If PARAM is set to unity, (1.0) shell thickness offsets are ignored, and the orientation of the shell surfaces is re- quired such that the outward normals point to the op- posing contact surface. EQ.3: as 1 above but with failure after sticking. EQ.4: EQ.5: tiebreak is active for nodes which are initially in contact but tangential motion with frictional sliding is permit- ted. tiebreak is active for nodes which are initially in contact. Stress is limited by the yield condition de- scribed in Remark 5 below. Damage behavior is mod- eled by a curve which defines normal stress vs. gap (crack opening). This option can be used to represent deformable glue bonds. EQ.6: This option is for use with solids and thick shells only. Tiebreak is active for nodes which are initially in con- tact. Failure stress must be defined for tiebreak to oc- cur. After the failure stress tiebreak criterion is met, damage is a linear function of the distance C between VARIABLE DESCRIPTION points initially in contact. When the distance is equal to PARAM, damage is fully developed and interface fail- ure occurs. After failure, this option behaves as a sur- face-to-surface contact. EQ.7: Dycoss Discrete Crack Model. “…_ONE_WAY_SUR- FACE_TO_SURFACE_TIEBREAK” definition is rec- ommended for this option. See Remarks. EQ.8: This is similar to OPTION = 6, but it works with offset shell elements. “…_ONE_WAY_SURFACE_TO_SUR- FACE_TIEBREAK” definition is recommended for this option. EQ.9: Discrete Crack Model with power law and B-K damage models. “…_ONE_WAY_SURFACE_TO_SURFACE_- TIEBREAK” definition is recommended for this option. See Remarks. EQ.10: This is similar to OPTION = 7, but it works with offset shell elements. “…_ONE_WAY_SURFACE_TO_SUR- FACE_TIEBREAK” definition is recommended for this option. EQ.11: This is similar to OPTION = 9, but it works with offset shell elements. “…_ONE_WAY_SURFACE_TO_SUR- FACE_TIEBREAK” definition is recommended for this option. Normal failure stress for OPTION = 2, 3, 4, 6, 7, 8, 9, 10 or 11. For OPTION = 5 NFLS becomes the plastic yield stress as defined in Remark 5. For OPTION = 9 or 11 and NFLS < 0, a load curve ID = -NFLS is referenced defining normal failure stress as a function of element size. See remarks. Shear failure stress for OPTION = 2, 3, 6, 7, 8, 9, 10 or 11. For OPTION = 4, SFLS is a frictional stress limit if PARAM = 1. This frictional stress limit is independent of the normal force at the tie. For OPTION = 5 SFLS becomes the curve ID which defines normal stress vs. gap. For OPTION = 9 or 11 and SFLS < 0, a load curve ID = -SFLS is referenced defining shear failure stress as a function of element size. See remarks. NFLS SFLS PARAM For OPTION = 2, setting PARAM = 1 causes the shell thickness offsets to be ignored. For OPTION = 4, setting PARAM = 1 causes SFLS to be a frictional stress limit. For OPTION = 6 or 8, VARIABLE DESCRIPTION ERATEN ERATES CT2CN CN PARAM is the critical distance, CCRIT, at which the interface failure is complete. For OPTION = 7 or 10 PARAM is the friction angle in degrees. For OPTION = 9 or 11, it is the exponent in the damage model. A positive value invokes the power law, while a negative one, the B-K model. See MAT_138 for additional details. For OPTION = 7, 9, 10, 11 only. Normal energy release rate (stress × length) used in damage calculation, see Lemmen and Meijer [2001]. For OPTION = 7, 9, 10, 11 only. Shear energy release rate (stress × length) used in damage calculation, see Lemmen and Meijer [2001]. The ratio of the tangential stiffness to the normal stiffness for OPTION = 9, 11. The default is 1.0. Normal stiffness (stress/length) for OPTION = 9, 11, and OPTION = 7 for the MORTAR option only. If CN is not given explicitly, penalty stiffness divided by segment area is used (default). This optional stiffness should be used with care, since contact stability can get affected. A warning message with a recommended time step is given initially. DMP_1 Mode I damping force per unit velocity per unit area. DMP_2 Mode II damping force per unit velocity per unit area. DMP_3 Mode III damping force per unit velocity per unit area. Remarks: 1. After failure, this contact option behaves as a surface-to-surface contact with thickness offsets. After failure, no interface tension is possible. 2. The soft constraint option with SOFT = 2 is not implemented for the tiebreak option. 3. For OPTION = 2, 3, and 6 the tiebreak failure criterion has normal and shear components: ( |𝜎𝑛 | NFLS ) + ( ∣𝜎𝑠∣ SFLS ) ≥ 1. 4. For OPTION = 4, the tiebreak failure criterion has only a normal stress component: |𝜎𝑛| NFLS ≥ 1. 5. For OPTION = 5, the stress is limited by a perfectly plastic yield condition. For ties in tension, the yield condition is For ties in compression, the yield condition is √𝜎𝑛 2 + 3∣𝜎𝑠∣2 NLFS ≤ 1. √3∣𝜎𝑠∣2 NLFS ≤ 1. The stress is also scaled by the damage function which is obtained from the load curve. For ties in tension, both normal and shear stress are scaled. For ties in compression, only shear stress is scaled. 6. For OPTION = 6 or 8, damage initiates when the stress meets the failure criterion. The stress is then scaled by the damage function. Assuming no load reversals, the energy released due to the failure of the interface is approximate- ly 0.5 × S × CCRIT, where 𝑆 = √max(𝜎𝑛, 0)2 + ∣𝜎𝑠∣2 at the initiation of damage. This interface may be used for simulating crack propagation. For the energy release to be correct, the contact penalty stiffness must be much larger than min(NFLF, SFLS) . CCRIT 7. OPTION = 7 or 10 is the Dycoss Discrete Crack Model as described in Lemmen and Meijer [2001]. The relation for the crack initiation is given as [ max(𝜎𝑛, 0) NFLS ] + [ 𝜎𝑠 SFLS − sin(PARAM)min(0, 𝜎𝑛) ] = 1. 8. OPTION = 9 or 11 is based on the fracture model in the cohesive material model *MAT_COHESIVE_MIXED_MODE, where the model is described in detail. Failure stresses/peak tractions NFLS and/or SFLS can be defined as functions of characteristic element length (square root of master segment area) via load curve. This option is useful to get nearly the same global responses (e.g. load- displacement curve) with coarse meshes compared to a fine mesh solution. In general, lower peak tractions are needed for coarser meshes. See also *MAT_- 138. 9. For OPTIONs 6 thru 11 of *CONTACT_AUTOMATIC_ONE_WAY_SUR- FACE_TO_SURFACE_TIEBREAK, one can determine the condition of the tie- break surface via the component labeled "contact gap" in the intfor database (*DATABASE_BINARY_INTFOR). The "contact gap" actually represents a damage value ranging from 0 (tied, no damage) to 1 (released, full damage). 10. Tying in the AUTOMATIC_..._TIEBREAK contacts occurs if the slave node is within a small tolerance of the master surface after taking into account contact thicknesses. For MPP, the tolerance is given by tol = 0.01√2 × master segment area for SMP, the tolerance is 0.4(slave contact thickness + master contact thickness). 11. It is recommended that the slave and master sides of tiebreak contact be defined using segment sets rather than part IDs or part set IDs. In this way, the user can be more selective in choosing which segments are to be tied and ensure that contact stresses calculated from nodal contact forces are not diluted by seg- ments that are not actually on the actual contact surface. The user also has direct control over the contact segment normal vectors when segment sets are used. Segment normal vectors should point toward the opposing contact sur- face so that tension is properly distinguished from compression. Card 4: AUTOMATIC_SURFACE_TO_SURFACE_COMPOSITE This card 4 is mandatory for: *CONTACT_AUTOMATIC_SURFACE_TO_SURFACE_COMPOSITE Card 4a 1 2 3 4 Variable TFAIL MODEL CIDMU CIDETA Type F I I I 5 D F Default required required required required 0.0 6 7 VARIABLE DESCRIPTION TFAIL Tensile traction 𝜎𝑓 required for failure. MODEL Model for shear response. See the equations in the Remarks for details. EQ.1: limiting shear stress depends on CIDMU in both tension and compression. See remark 3. EQ.2: limiting shear stress depends on CIDETA in tension and CIDMU in compression. See remark 4. EQ.3: limiting shear stress depends on CIDETA in both tension and compression. See remark 5. CIDMU Curve ID for the coefficient of friction 𝜇(𝐻) as a function of the Hershey number 𝐻. CIDETA Curve ID for the viscosity 𝜂(𝑇) as a function of temperature 𝑇. D Composite film thickness. Remarks: 1. This contact model is designed for simulating the processing of laminated composite materials. Surfaces in contact may support shear up to the limit defined by MODEL and be in compression or in tension up to the tensile limit 𝜎𝑓 defined by TFAIL. After TFAIL is reached, the contact fails in both tension and shear. If the surfaces come back into contact, the bonding heals, and the contacting surfaces may support shear and tension. 2. The viscosity 𝜂(𝑇) is defined as a function of temperature by CIDETA. The value of the viscosity is not extrapolated if the temperature falls outside of the temperature range defined by the curve. 3. The coefficient of friction 𝜇 for MODEL = 1 is defined in terms of the Hershey number 𝐻 = 𝜂(𝑇)𝑉/(𝑝 + 𝜎𝑓 ) where p is the contact pressure (positive in com- pression, and negative in tension) and V the relative velocity between the sur- faces. 𝜏 ≤ μ(𝐻)(𝑝 + 𝜎𝑓 ) 4. The coefficient of friction 𝜇 for MODEL = 2 is defined in terms of the Hershey number 𝐻 = 𝜂(𝑇)𝑉/𝑝. Note the definition of the Hershey number for this model differs from MODEL = 1. In compression the shear stress is limited by 𝜏 ≤ μ(𝐻)𝑝 and in tension, the shear stress is limited according to 𝜏 ≤ 𝜂(𝑇)𝑉/𝑑 5. The shear stress for MODEL = 3 in tension and compression is limited according to 𝜏 ≤ 𝜂(𝑇)𝑉/𝑑. Card 4: SINGLE_SURFACE_TIED This card 4 is mandatory for: *CONTACT_AUTOMATIC_SINGLE_SURFACE_TIED Card 4 1 2 3 4 5 6 7 8 Variable CLOSE Type F Default 0.0 VARIABLE CLOSE Remarks: DESCRIPTION Surfaces closer than CLOSE are tied. If CLOSE is left as 0.0, it is defaulted to one percent of the mesh characteristic length scale. Nodes that are above or below the surface will be tied if they are close enough to the surface. This special feature is implemented to allow for the calculation of eigenvalues and eigenvectors on geometries that are connected by a contact interface using the AUTO- MATIC_SINGLE_SURFACE options. If there is significant separation between the tied surfaces, the rigid body modes will be opposed by the contact stiffness, and the calculated eigenvalues for rigid body rotations will not be zero. Card 4: AUTOMATIC_SURFACE_TO_SURFACE_TIED_WELD This card 4 is mandatory for: *CONTACT_AUTOMATIC_SURFACE_TO_SURFACE_TIED_WELD Card 4 1 2 3 4 5 6 7 8 Variable TEMP CLOSE Type F F Default None 0.0 DESCRIPTION Minimum temperature required on both surfaces for tying. Once the surfaces are tied, they remain tied even if the temperature drops. Surfaces closer than CLOSE are tied. If CLOSE is left as 0.0, it is defaulted to one percent of the mesh characteristic length scale. Nodes that are above or below the surface will be tied if they are close enough to the surface. VARIABLE TEMP CLOSE Remarks: This special feature is implemented to allow for the simulation of welding. As regions of the surfaces are heated to the welding temperature and come into contact, the nodes are tied. If there is significant separation between the tied surfaces, the rigid body modes will not be opposed by the contact stiffness. In other words, the offset between the surfaces is handled like the contact with OFFSET. If the surfaces are below the welding temperature, the surfaces interact with the standard AUTOMATIC_SURFACE_TO_SURFACE options. Card 4: CONSTRAINT_…_TO_SURFACE This card 4 is mandatory for: *CONTACT_CONSTRAINT_NODES_TO_SURFACE *CONTACT_CONSTRAINT_SURFACE_TO_SURFACE Card 4 1 2 3 4 5 6 7 8 Variable KPF Type F Default 0.0 VARIABLE DESCRIPTION KPF Kinematic partition factor for constraint: EQ.0.0: fully symmetric treatment. EQ.1.0: one way treatment with slave nodes constrained to master surface. Only the slave nodes are checked against contact. EQ.-1.0: one way treatment with master nodes constrained to slave surface. Only the master nodes are checked against contact. Card 4: DRAWBEAD This card 4 is mandatory for: *CONTACT_DRAWBEAD *CONTACT_DRAWBEAD_INITIALIZE Note variables related to automatic multiple draw bead feature, including NBEAD, POINT1, POINT2, WIDTH, and EFFHGT are not applicable to *CONTACT_DRAW- BEAD_INITIALIZE. Card 4a 1 2 3 4 5 6 7 8 Variable LCIDRF LCIDNF DBDTH DFSCL NUMINT DBPID ELOFF NBEAD Type I I F F Default required none 0.0 1.0 I 0 I 0 I 0 I none Additional card to be included if NBEAD is defined. Card 4b 1 2 3 4 5 6 7 8 Variable POINT1 POINT2 WIDTH EFFHGT Type I I F F Default none none none none = Ffriction + Fbending DBDTH Figure 11-2. The draw bead contact model. Initialization Card. Additional card for INITIALIZE keyword option. Card to initialize the plastic strain and thickness of elements that pass under the draw bead. Card 4c 1 2 3 4 5 6 7 8 Variable LCEPS TSCALE LCEPS2 OFFSET Type I F I F Default required 1.0 optional optional VARIABLE LCIDRF LCIDNF DESCRIPTION If LCIDRF is positive then it defines the load curve ID giving the bending component of the restraining force, Fbending, per unit draw bead length as a function of displacement, 𝛿, see Figure 11-2. This force is due to the bending and unbending of the blank as it moves through the draw bead. The total restraining force is the sum of the bending and friction components. If LCIDRF is negative, then the absolute value gives the load curve ID defining max bead force versus normalized draw bead length. The abscissa values are between zero and 1 and are the normalized draw bead length. The ordinate gives the maximum allowed draw bead, retaining force when the bead is in the fully closed position. If the draw bead is not fully closed, linear interpolation is used to compute the draw bead force. Load curve ID giving the normal force per unit draw bead length as a function of displacement, 𝛿, see Figure 11-2. This force originates from bending the blank into the draw bead as the binder closes on the die. The normal force begins to develop when the distance between the die and binder is less than the draw bead depth. As the binder and die close on the blank this force should diminish or reach a plateau. DBDTH DFSCL NUMINT DBPID ELOFF *CONTACT_OPTION1_{OPTION2}_… DESCRIPTION Draw bead depth, see Figure 11-2. Necessary to determine correct 𝛿 displacement from contact displacements. Scale factor for load curve. Default = 1.0. This factor scales load curve ID, LCIDRF above. Number of equally spaced integration points along the draw bead: EQ.0: Internally calculated based on element size of elements that interact with draw bead. This is necessary for the correct calculation of the restraining forces. More integration points may increase the accuracy since the force is applied more evenly along the bead. Optional part ID for the automatically generated truss elements for the draw bead display in the post-processor. If undefined LS- DYNA assigns a unique part ID. Option to specify and element ID offset for the truss elements that are automatically generated for the draw bead display. If undefined LS-DYNA chooses a unique offset. NBEAD Number of line beads in odd integer. POINT1 Node ID of the first node on a binder. POINT2 Node ID of a matching node on the opposing binder. WIDTH EFFHGT LCEPS Total bead width defining distance between inner and outer most bead walls. Effective bead height. Draw bead restraining force starts to take effect when binder gap is less than EFFHGT. through thickness. the shell Load curve ID defining the plastic strain versus the parametric coordinate The parametric coordinate should be defined in the interval between -1 and 1 inclusive. The value of plastic strain at the integration point is interpolated from this load curve. If the plastic strain at an integration point exceeds the value of the load curve at the time initialization occurs, the plastic strain at the point will remain unchanged. VARIABLE TSCALE LCEPS2 DESCRIPTION Scale factor that multiplies the shell thickness as the shell element moves under the draw bead. Optional load curve ID defining the plastic strain versus the parametric coordinate through the shell thickness, which is used after an element has traveled a distance equal to OFFSET. The parametric coordinate should be defined in the interval between - 1 and 1 inclusive. The value of plastic strain at the integration point is interpolated from this load curve. If the plastic strain at an integration point exceeds the value of the load curve at the time initialization occurs, the plastic strain at the point will remain unchanged. Input parameters LCEPS2 and OFFSET provides a way to model the case where a material moves under two draw beads. In this latter case the curve would be the sum of the plastic strains generate by moving under two consecutive beads. OFFSET If the center of an element has moved a distance equal to OFFSET, the load curve ID, LCEPS2 is used to reinitialize the plastic strain. The TSCALE scale factor is also applied. Overview: In the framework of this draw bead model the blank is the master part, and the male part of the draw bead is the slave. The male part of the draw bead, which moves with the punch, is input as a curve defined using a list of nodes or a part consisting of beams, as discussed below. Associated with this curve is a region of influence that is characterized by the DBDTH field of card 4a. As the punch comes down and the region of influence intersects the elements on the blank, forces are applied to the blank at the points of closest approach. These forces depend on the separation distance, 𝛿, which is geometrically defined in Figure 11-2. The draw bead force model consists of two terms: 6. There is a resisting force, which is a function of 𝛿, and is defined through the load curve specified in the LCIDRF field. This force is applied in a direction opposite to velocity. 7. There is also a normal force pushing the male part of the draw bead away from the blank, which is specified by LCIDNF. This normal force, in turn, is used to model friction, which depends on the product of the friction coefficient and the normal force. The curve representing the male part of the draw bead can be defined in three ways: 1. A consecutive list of slave nodes that lie along the bead. 2. A part ID of a beam that lies along the draw bead. 3. A part set ID of beams that lie along the draw bead. For straight draw beads, only two nodes or a single beam needs to be defined, i.e., one at each end. For curved beads, many nodes or beams may be required to define the curvature of the bead geometry. When beams are used to define the bead, with the exception of the first and last node, each node must connect with two beam elements. This requirement means that the number of slave nodes equals the number of beam elements plus one. It is at the integration points where the contact algorithm checks for penetration. Integration points are equally spaced along the draw bead and do not depend on the nodal spacing used in the definition of the draw bead. By using the capability of tying extra nodes to rigid bodies the draw bead nodal points do not need to belong to the element connectivities of the die and binder. The blank makes up the master surface. NOTE: It is highly recommended to define a BOXID around the draw bead to limit the size of the master surface considered for the draw bead. This will substantially reduce cost and memory requirements. LS-PrePost: While defining a contact draw bead may involve several keywords, the processed is streamlined by the “draw bead” definition feature of LS-PrePost4.0’s eZ-Setup for metal forming application. See, http://ftp.lstc.com/anonymous/outgoing/lsprepost/4.0/metalforming/ Multiple draw beads model: Developed in conjunction with the Ford Motor Company Research & Advanced Engineering Laboratory, the multiple draw bead features provides a simple way to model (1) the neglected effects of the draw bead width, and (2) to attenuate the bead forces when the distance between upper and lower binders is more than the draw bead height. 1. Draw Bead Width Correction. As shown in Figure 11-3, it often happens that a sheet blank edge does not cross the draw bead’s curve of definition but does fall within its width. When the bead is modelled as a 1-dimensional (no width) curve, it is possible that a major portion of the blank would have no forces applied, while, in reality, there are still two bending radii at the inner bead wall providing about 50% of the total bead forces. The neglect of width effects leads to excessive blank edge draw-ins resulting in either loose metal in the part, or wrinkles on the draw wall or product surface. The multiple beads feature ameliorates this particular shortcoming by replacing the single 1-dimensional bead with an equivalent set of beads distributed over the width of the physical bead. The bead force is distributed uniformly over the NBEAD sub-beads, such that the resultant force is equal to that of the original 1-dimensionsal bead. Note that NBEAD must be an odd integer. Figure 11-4 schematically represents the NBEAD = 3 case for which two addi- tional line beads are automatically generated. The forces specified by the load curve, LCIDRF, will be evenly distributed over the 3 beads. In Figure 11-5, bead forces are recovered from the ASCII rcforc files for both cases of NBEAD = 1 and 3, indicating the total force applied (shown on the left) on one single bead is distributed evenly among the three automatically generated beads for the case of NBEAD = 3. The stress distribution is also more realistic with the multiple beads. In a chan- nel draw (half model) as shown in Figure 11-9, no significant changes in mean stress values are found between NBEAD = 3 and one single line bead. In fact, the compressive stresses are more realistically and evenly distributed around the bead region, with stresses in NBEAD = 3 about 1/3 of those in one line bead. 2. Lower Binder Gap Correction. As originally implemented, the draw bead contact model applies the draw bead forces, as specified in the load curve, when the upper binder reaches the blank, regardless of the lower binder’s posi- tion. If the lower binder is not in contact with the blank, LS-DYNA still applies draw bead forces, even though it is unphysical to do so. The EFFHGT, POINT1 and POINT2 fields together provide a simple model to avoid these unphysical forces. The POINT1 and POINT2 fields are taken as nodes on the opposing binders. The draw bead contact is disabled when the Euclidean distance be- tween POINT1 and POINT2 is greater than EFFHGT; consequently, the two nodes must be chosen so they converge to a single point as the draw bead clos- es. As shown in Figure 11-6, a simple model was built to verify the effectiveness of the variable EFFHGT. The upper binder is pushed down to close with the low- er binder while a strip of sheet blank is being pulled in the direction indicated. The distance between the binders is 12mm initially, as shown in Figure 11-7, and the closing gap and pulling force in x were recovered throughout the simu- lation. With the EFFHGT set at 8mm, the pulling force history indicates the bead forces starting to take effect after the upper binder has traveled for 4mm, Figure 11-8, as expected. Revision information: The NBEAD feature is available in LS-DYNA R6 Revision 69556 and later releases, with important updates in Revision 79270. Inner bead wall Blank edge flow direction Blank drawn edge Outer bead wall Location of a single line bead force Figure 11-3. A possible scenario of sheet blank edge draw-in condition. Auto-created beads Defined node set/beam WIDTH 5.25 5.25 EFFHGT Figure 11-4. Definition of multiple draw beads. ) ( 14 12 10 -2 0.002 0.004 min=-7.3006 max=13559 ~13559N Legend rcforc bead 1 0.008 0.01 0.006 Time ) ( -1 0.002 0.004 min=27.946 max=4523.8 ~4523N Legend rcforc bead 1 rcforc bead 2 rcforc bead 3 0.008 0.01 0.006 Time Figure 11-5. Bead force verification between NBEAD = 1 (left) and 3. Bead #3 Bead #5 Bead #4 (Beads attached to the upper binder) Details in next figure Figure 11-6. A verification model for the variable EFFHGT. POINT1(node) Draw beads Sheet strip Upper binder 12mm Tracking binder closing gap as abscissa values Pull in X Tracking the pulling force in X as ordinate values POINT2 (node) Lower binder Figure 11-7. Tracking the closing gap and pulling distance. 200 150 100 50 ) ( -50 -12 Bead force starts taking effect at a distance of 8.0mm -10 -8 -6 -4 -2 Closing distance (mm) Figure 11-8. Pulling force (NODFOR) vs. closure distance. Time=0.0152, #nodes=7005, #elem=6503 Contours of pressure (mid-plane) min=-395.339, at elem# 15423 max=28.1887, at elem# 13317 Time=0.0152, #nodes=6976, #elem=6476 Contours of pressure (mid-plane) min=-401.24, at elem# 15280 max=74.6163, at elem# 13016 Pressure (MPa) 28.2 Pressure (MPa) 74.6 -14.2 -56.5 -98.9 -141.2 -183.6 -225.9 -268.3 -310.6 -353.0 -395.3 27.0 -20.6 -68.1 -115.7 -163.3 -210.9 -258.5 -306.1 -353.7 -401.2 Mean stresses of a channel draw (NBEAD=3) Mean stresses of a channel draw on one line bead Figure 11-9. Mean stress comparison between NBEAD = 3 and 1. Card 4: ERODING_..._SURFACE This card 4 is mandatory for: *CONTACT_ERODING_NODES_TO_SURFACE *CONTACT_ERODING_SINGLE_SURFACE *CONTACT_ERODING_SURFACE_TO_SURFACE Card 4 1 2 3 4 5 6 7 8 Variable ISYM EROSOP IADJ Type Default I 0 I 0 I 0 VARIABLE DESCRIPTION ISYM Symmetry plane option: EQ.0: off, EQ.1: do not include faces with normal boundary constraints (e.g., segments of brick elements on a symmetry plane). This option is important to retain the correct boundary conditions in the model with symmetry. EROSOP Erosion/Interior node option: (reset to 1 internally) EQ.0: only exterior boundary information is saved, EQ.1: storage is allocated so that eroding contact can occur. Otherwise, no contact is assumed after erosion of the corresponding element. IADJ Adjacent material treatment for solid elements: (reset to 1 internally) EQ.0: solid element faces are included only for free bounda- ries, EQ.1: solid element faces are included if they are on the boundary of the material subset. This option also allows the erosion within a body and the subsequent treatment of contact. *CONTACT_OPTION1_{OPTION2}_… Eroding contact may control the timestep . For ERODING_NODES_TO_SURFACE, define the slave side using a node set, not a part ID or part set ID. Use of an ERODING contact automatically invokes a negative volume failure criterion in for all solid elements *CONTROL_SOLID. Use of PSFAIL will limit the negative volume failure criterion to a set of solid parts. A negative volume failure criterion circumvents an error termination due to negative volume by deleting solid elements that develop negative volume. the model, except as overridden by PSFAIL in Contact friction is not considered by SMP LS-DYNA for *CONTACT_ERODING_- NODES_TO_SURFACE and *CONTACT_ERODING_SURFACE_TO_SURFACE unless SOFT is set to 2 on Optional Card A. MPP LS-DYNA has no such exclusion for contact friction. Values of EROSOP = 0 and IADJ = 0 are not supported, and both are reset to 1 internally. Card 4: SURFACE_INTERFERENCE This card 4 is mandatory for: *CONTACT_NODES_TO_SURFACE_INTERFERENCE *CONTACT_ONE_WAY_SURFACE_TO_SURFACE_INTERFERENCE *CONTACT_SURFACE_TO_SURFACE_INTERFERENCE Purpose: This contact option provides a means of modeling parts which are shrink fitted together and are, therefore, prestressed in the initial configuration. This option turns off the nodal interpenetration checks (which changes the geometry by moving the nodes to eliminate the interpenetration) at the start of the simulation and allows the contact forces to develop to remove the interpenetrations. The load curves defined in this section scale the interface stiffness constants such that the stiffness can increase slowly from zero to a final value with effect that the interface forces also increase gradually to remove the overlaps. Card 4 1 2 3 4 5 6 7 8 Variable LCID1 LCID2 Type Default I 0 I 0 DESCRIPTION Load curve ID which scales the interface stiffness during dynamic relaxation. This curve must originate at (0, 0) at time = 0 and gradually increase. Load curve ID which scales the interface stiffness during the transient calculation. This curve generally has a constant value of unity for the duration of the calculation if LCID1 is defined. If LCID1 = 0, this curve must originate at (0, 0) at time = 0 and gradually increase to a constant value. VARIABLE LCID1 LCID2 Remarks: 1. Shell thickness offsets are taken into account for deformable shell elements. 2. The check to fix initial penetrations is skipped. 3. Automatic orientation of shell elements is skipped. 4. Furthermore, segment orientation for shell elements and interpenetration checks are skipped. Therefore, it is necessary in the problem setup to ensure that all contact segments which belong to shell elements are properly oriented, i.e., the outward normal vector of the segment based on the right hand rule relative to the segment numbering, must point to the opposing contact surface; consequently, automatic contact generation should be avoided for parts composed of shell elements unless automatic generation is used on the slave side of a nodes to surface interface. Card 4: RIGID_TO_RIGID This card 4 is mandatory for: *CONTACT_RIGID_NODES_TO_RIGID_BODY *CONTACT_RIGID_BODY_ONE_WAY_TO_RIGID_BODY *CONTACT_RIGID_BODY_TWO_WAY_TO_RIGID_BODY Card 4 1 2 Variable LCID FCM Type I I 3 US F 4 5 6 7 8 LCDC DSF UNLCID I F I Default required required LCID optional 0.0 optional VARIABLE LCID DESCRIPTION Load curve ID giving force versus penetration behavior for RIGID_contact. See also the definition of FCM below. FCM Force calculation method for RIGID_contact: EQ.1: Load curve gives total normal force on surface versus maximum penetration of any node (RIGID_BODY_- ONE_WAY only). EQ.2: Load curve gives normal force on each node versus penetration of node through the surface (all RIG- ID_contact types). EQ.3: Load curve gives normal pressure versus penetration of node through the surface (RIGID_BODY_TWO_WAY and RIGID_BODY_ONE_WAY only). EQ.4: Load curve gives total normal force versus maximum soft penetration. In this case the force will be followed based on the original penetration point. (RIGID_- BODY_ONE_WAY only). US Unloading stiffness for RIGID_contact. The default is to unload along the loading curve. This should be equal to or greater than the maximum slope used in the loading curve. Loading Curve Unloading Stiffness Unloading Curve Penetration VARIABLE LCDC Figure 11-10. Behavior if an unloading curve is defined DESCRIPTION (DC) versus ID giving damping coefficient Load curve penetration velocity. The damping force FD is then: FD = DSF × DC × velocity. DSF Damping scaling factor. UNLCID Optional load curve ID giving force versus penetration behavior for RIGID_BODY_ONE_WAY contact. This option requires the definition of the unloading stiffness, US. See Figure 11-10. Card 4: TIEBREAK_NODES This card 4 is mandatory for: *CONTACT_TIEBREAK_NODES_TO_SURFACE and *CONTACT_TIEBREAK_NODES_ONLY Card 4 1 2 3 4 5 6 7 8 Variable NFLF SFLF NEN MES Type F F F Default required required 2. F 2. VARIABLE DESCRIPTION Normal failure force. Only tensile failure, i.e., tensile normal forces, will be considered in the failure criterion. Shear failure force Exponent for normal force Exponent for shear force. Failure criterion: ( ∣𝑓𝑛∣ NFLF NEN ) + ( ∣𝑓𝑠∣ SFLF MES ) ≥ 1. Failure is assumed if the left side is larger than 1. 𝑓𝑛 and 𝑓𝑠 are the normal and shear interface force. NFLF SFLF NEN MES Remarks: These attributes can be overridden node by node on the *SET_NODE_option cards. Both NFLF and SFLF must be defined. If failure in only tension or shear is required then set the other failure force to a large value (1E+10). After failure, contact_tiebreak_nodes_to_surface behaves as a nodes-to-surface contact with no thickness offsets (no interface tension possible) whereas the contact_tiebreak_ nodes_only stops acting altogether. Prior to failure, the two contact types behave identically. Card 4: TIEBREAK_SURFACE This card 4 is mandatory for: *CONTACT_TIEBREAK_SURFACE_TO_SURFACE and *CONTACT_TIEBREAK_SURFACE_TO_SURFACE_ONLY Card 4 1 2 3 4 5 6 7 8 Variable NFLS SFLS TBLCID THKOFF Type F F I Default required required 0 I 0 VARIABLE DESCRIPTION NFLS SFLS Tensile failure stress. See remark below. Shear failure stress. Failure criterion ( |𝜎𝑛| NFLS ) + ( ) ∣𝜎𝑠∣ SFLS ≥ 1. Optional load curve number defining the resisting tensile stress versus gap opening in the normal direction for the post failure response. This option applies only to SMP and can be used to model adhesives. Thickness offsets are considered if THKOFF = 1. If shell offsets are included in the meshed geometry, this option is highly recommended since segment orientation can be arbitrary and the contact surfaces can be disjoint. This option is not available in the MPP version of LS-DYNA. It works by substituting *CON- TACT_AUTOMATIC_SURFACE_TO_SURFACE_TIEBREAK (OPTION = 2 if TBLCID is not specified; OPTION = 5 if TBLCID is specified). TBLCID THKOFF Remarks: The failure attributes can be overridden segment by segment on the *SET_SEGMENT or *SET_SHELL_option cards for the slave surface as A1 and A2. These variables do not apply to the master surface. Both NFLS and SFLS must be defined. If failure in only tension or shear is required then set the other failure stress to a large value (1E+10). When used with shells, contact segment normals are used to establish the tension direction (as opposed to compression). Compressive stress does not contribute to the failure equation. After failure, *CONTACT_TIEBREAK_SURFACE_TO_SURFACE behaves as a surface- to-surface contact with no thickness offsets. After failure, *CONTACT_TIEBREAK_SURFACE_TO_SURFACE_ONLY stops acting altogether. Until failure, it ties the slave nodes to the master nodes. Card 4: CONTRACTION_JOINT This card 4 is mandatory for: *CONTACT_SURFACE_TO_SURFACE_CONTRACTION_JOINT Purpose: This contact option turns on the contraction joint model designed to simulate the effects of sinusoidal joint surfaces (shear keys) in the contraction joints of arch dams and other concrete structures. The sinusoidal functions for the shear keys are defined according to the following three methods [Solberg and Noble 2002]: Method 1: Method 2: Method 3: (default) 𝑔̂ = 𝑔 − 𝐴{1 − cos[𝐵(𝑠2 − 𝑠1)]} 𝑔̂ = 𝑔 − 2𝐴 ∣sin [ 𝐵(𝑠2 − 𝑠1) ]∣ 𝑔̂ = 𝑔 − 𝐴cos(𝐵𝑠2) + 𝐴cos(𝐵𝑠1) Where 𝑔 is a gap function for contact surface, 𝑔̂ is gap function for the joint surface. 𝐴 is key amplitude parameter, and 𝐵 is key frequency parameter. 𝑠1 and 𝑠2 are referential surfaces: 𝑠1 = 𝐗surface1 ⋅ 𝐓key 𝑠2 = 𝐗surface2 ⋅ 𝐓key 𝐓key = 𝐓slide × 𝐧 Where 𝐓slide is the free sliding direction of the keys, 𝐧 is the surface normal in reference. Card 4 1 2 3 4 5 6 7 8 Variable MTCJ ALPHA BETA TSVX TSVY TSVZ Type Default I 0 F F F F F 0.0 0.0 0.0 0.0 0.0 VARIABLE DESCRIPTION MTCJ The method option for the gap function, 𝑔̂ ALPHA Key amplitude parameter A BETA TSVX TSVY TSVZ Key frequency parameter B 𝑥 component of the free sliding direction 𝐓slide 𝑦 component of the free sliding direction 𝐓slide 𝑧 component of the free sliding direction 𝐓slide *CONTACT_OPTION1_{OPTION2}_… This card is mandatory for the THERMAL option, i.e.: *CONTACT_…_THERMAL_… Reminder: If Card 4 is required, then it must go before this thermal card. (Card 4 is required for certain contact types - see earlier in this section for the list, later in this section for details of Card 4.) Thermal Card l. Card 1 Variable Type 1 K F 2 FRAD F 3 H0 F 4 5 6 7 8 LMIN LMAX FTOSLV BC_FLG ALGO F F F I 0 I 0 Default none none none none none 0.5 VARIABLE DESCRIPTION K Thermal conductivity of fluid between the contact surfaces. If a gap with a thickness 𝑙gap exists between the contact surfaces, then the conductance due to thermal conductivity between the contact surfaces is ℎcond = 𝑙gap Note that LS- DYNA calculates 𝑙gap based on deformation FRAD Radiation factor between the contact surfaces. Where, 𝑓rad = + 1 𝜀2 𝜀1 − 1 𝜎 = Stefan-Boltman constant 𝜀1 = emissivity of master surface 𝜀2 = emissivity of slave surface LS-DYNA calculates a radiant heat transfer conductance ℎrad = 𝑓rad(𝑇𝑚 + 𝑇𝑠)(𝑇𝑚 2 + 𝑇𝑠 2) VARIABLE H0 DESCRIPTION Heat transfer conductance for closed gaps. Use this heat transfer conductance for gaps in the range 0 ≤ 𝑙gap ≤ 𝑙min LMIN Minimum gap, 𝑙min, use the heat transfer conductance defined (H0) for gap thicknesses less than this value. If 𝑙min < 0, then −𝑙min is a load curve number defining 𝑙min as a function time. LMAX No thermal contact if gap is greater than this value (𝑙max). FTOSLV Fraction, 𝑓 , of sliding friction energy partitioned to the slave surface. Energy partitioned to the master surface is (1 − 𝑓 ). EQ.0: Default set to 0.5: The is sliding partitioned 50% - 50% to the slave and master surfaces in contact. friction energy 𝑓 = . √(𝜌𝐶𝑝𝑘) 1 + master side material √(𝜌𝐶𝑝𝑘) slave side material BC_FLAG Thermal boundary condition flag EQ.0: thermal boundary conditions are on when parts are in contact EQ.1: thermal boundary conditions are off when parts are in contact ALGO Contact algorithm type. EQ.0: two way contact, both surfaces change temperature due to contact EQ.1: one way contact, master surface does not change temperature due to contact. Slave surface does change temperature. Remarks: Note that LS- DYNA calculates 𝑙gap based on deformation *CONTACT_OPTION1_{OPTION2}_… ℎ = ⎧ℎ0 {{ ℎcond + ℎrad ⎨ {{ ⎩ 0 ≤ 𝑙gap ≤ 𝑙min 𝑙min < 𝑙gap ≤ 𝑙max 𝑙gap > 𝑙max THERMAL FRICTION: This card is required if the FRICTION suffix is added to THERMAL. *CONTACT_…_THERMAL_FRICTION_… The blank (or work piece) must be defined as the slave surface in a metal forming model. Purpose: 1. Used to define the mechanical static and dynamic friction coefficients as a function of temperature. 2. Used to define the thermal contact conductance as a function of temperature and pressure. Card 1 1 2 3 Variable LCFST LCFDT FORMULA Type Default I 0 I 0 I 0 4 A I 0 5 B I 0. 6 C I 0 7 D I 0 8 LCH I 0 User Subroutine Cards. Additional cards for when FORMULA is a negative number. Use as many cards as necessary to set |FORMULA| number of parameters. Card 2 1 2 3 4 5 6 7 8 Variable UC1 UC2 UC3 UC4 UC5 UC6 UC7 UC8 Type F F F F F F F F Default 0.0 0.0 0.0 0.0 0.0 0.0 0.0 0.0 VARIABLE LCFST DESCRIPTION Load curve number for static coefficient of friction as a function of temperature. The load curve value multiplies the coefficient value FS. LCFDT *CONTACT_OPTION1_{OPTION2}_… DESCRIPTION Load curve number for dynamic coefficient of friction as a function of temperature. The load curve value multiplies the coefficient value FD. FORMULA Formula that defines the contact heat conductance as a function of temperature and pressure. EQ.1: ℎ(𝑃) is defined by load curve A, which contains data for contact conductance as a function of pressure. EQ.2: ℎ(𝑃) is given by the following where A, B, C and D although defined by load curves are typically constants for use in this formula. The load curves are to given as functions of temperature. ℎ(𝑃) = 𝑎 + 𝑏𝑃 + 𝑐𝑃2 + 𝑑𝑃3 EQ.3: ℎ(𝑃) is given by the following formula from [Shvets and Dyban 1964]. ℎ(𝑃) = 𝜋𝑘gas 4𝜆 [1. +85 ( 0.8 ) ] = [1. +85 ( 0.8 ) ] where, a: is evaluated from the load curve, A, for the thermal conductivity, 𝑘gas, of the gas in the gap as a function of temperature. b: is evaluated from the load curve, B, for the parameter grouping 𝜋/4𝜆. Therefore, this load curve should be set to a constant value. 𝜆 is the surface roughness. c: is evaluated from the load curve, C , which specifies a stress metric for deformation (e.g., yield) as a function of temperature. EQ.4: ℎ(𝑃) is given by the following formula from [Li and Sellars 1996]. where, ℎ(𝑃) = 𝑎 [1 − exp (−𝑏 )] 𝑎: is evaluated from the load curve, A, which defines a load curve as a function of temperature. 𝑏: is evaluated from the load curve, B, which defines a load curve as a function of temperature. VARIABLE DESCRIPTION A B C D LCH 𝑐: is evaluated from the load curve, C, which defines a stress metric for deformation (e.g., yield) as a function of temperature. 𝑑: is evaluated from the load curve D, which is a func- tion of temperature. EQ.5: ℎ(gap) is defined by load curve A, which contains data for contact conductance as a function of interface gap. LT.0: This is equivalent to defining the keyword *USER_IN- TERFACE_CONDUCTIVITY and the user subroutine usrhcon will be called for this contact interface for defin- ing the contact heat transfer coefficient. Load curve number for the 𝑎 coefficient used in the formula. Load curve number for the 𝑏 coefficient used in the formula. Load curve number for the 𝑐 coefficient used in the formula. Load curve number for the 𝑑 coefficient used in the formula. Load curve number for ℎ. This parameter can refer to a curve ID or a function ID . When LCH is a curve ID (and a function ID) it is interpreted as follows: GT.0: the heat transfer coefficient is defined as a function of time, 𝑡, by a curve consisting of (𝑡, ℎ(𝑡)) data pairs. LT.0: the heat transfer coefficient is defined as a function of temperature, 𝑇, by a curve consisting of (𝑇, ℎ(𝑇)) data pairs. When the reference is to a function it is prototyped as follows ℎ = ℎ(𝑡, 𝑇avg, 𝑇slv, 𝑇msr, 𝑃, 𝑔) where: 𝑡 = solution time 𝑇avg = average interface temperature 𝑇slv = slave segment temperature 𝑇msr = master segment temperature 𝑃 = interface pressure 𝑔 = gap distance between master and slave segment *CONTACT_OPTION1_{OPTION2}_… Additional cards for the ORTHO_FRICTION keyword option: *CONTACT_…_ORTHO_FRICTION_… Card 1 1 2 3 4 5 6 7 8 Variable FS1_S FD1_S DC1_S VC1_S LC1_S OACS_S LCFS LCPS Type F Default 0. F 0. F 0. F 0. Card 2 1 2 3 4 I 0 5 I 0 6 I 0 7 I 0 8 Variable FS2_S FD2_S DC2_S VC2_S LC2_S Type F Default 0. Card 3 1 F 0. 2 F 0. 3 F 0. 4 I 0 5 6 7 8 Variable FS1_M FD1_M DC1_M VC1_M LC1_M OACS_M LCFM LCPM Type F Default 0. F 0. F 0. F 0. I 0 I 0 I 0 I Card 4 1 2 3 4 5 6 7 8 Variable FS2_M FD2_M DC2_M VC2_M LC2_M Type F Default 0. F 0. F 0. F 0. I 0 VARIABLE FSn_S or M DESCRIPTION Static coefficient of friction in the local n orthotropic direction for the slave (S) or master (M) surface. The frictional coefficient is assumed to be dependent on the relative velocity 𝑣rel of the surfaces in contact, 𝜇𝑐 = FD + (FS − FD)𝑒−DC∣𝑣rel∣ where the direction and surface are left off for clarity. The OR- THO_FRICTION option applies to contact types: AUTOMATIC_SURFACE_TO_SUFACE, AUTOMATIC_ONE_WAY_SURFACE_TO_SURFACE, when they are defined by segment sets. specification of an offset angle in degrees from the 1-2 side which locates the 1 direction. The offset angle is input as the first attribute of the segment in *SET_SEGMENT. The transverse direction, 2, is in the plane of the segment and is perpendicular to the 1 direction. Each segment in the set FDI_S or M Dynamic coefficient of friction in the local n orthotropic direction. DCn_S or M Exponential decay coefficient for the local n direction. VCn_S or M Coefficient for viscous friction in the local n direction. See the description for VC for mandatory Card 2 above. LCn_S or M *CONTACT_OPTION1_{OPTION2}_… DESCRIPTION The table ID of a two dimensional table, see *DEFINE_TABLE or *DEFINE_TABLE_2D, giving the friction coefficient in the local n direction as a function of the relative velocity and interface pressure. In this case, each curve in the table definition defines the coefficient of interface pressure corresponding to a particular value of the relative velocity. friction versus the OACS_S or M LCFS or M If the default value, 0, is active, the frictional forces acting on a node sliding on a segment are based on the local directions of the segment. If OACS is set to unity, 1, the frictional forces acting on a node sliding on a segment are based on the local directions of the sliding node. No matter what the setting for OACS, the_S coefficients are always used for slave nodes and the_M coefficients for master nodes. Optional load curve that gives the coefficient of friction as a function of the direction of relative motion, as measured in degrees from the first orthotropic direction. If this load curve is specified, the other parameters (FS, FD, DC, VC, LC) are ignored. This is currently only supported in the MPP version. LCPS or M Optional load curve that gives a scale factor for the friction coefficient as a function of interface pressure. This is only used if LCFS (or M) is defined. Optional Card A: Reminder: If Card 4 is required, then it must go before this optional card. (Card 4 is required for certain contact types - see earlier in this section for the list.) Optional Card A. Optional 1 2 3 4 5 6 7 8 Variable SOFT SOFSCL LCIDAB MAXPAR SBOPT DEPTH BSORT FRCFRQ Type Default I 0 F .1 I 0 F F 1.025 0. I 2 I 10-100 I 1 Remarks type a13 VARIABLE DESCRIPTION SOFT Soft constraint option: EQ.0: penalty formulation, EQ.1: soft constraint formulation, EQ.2: segment-based contact. EQ.4: constraint approach for FORMING contact option. EQ.6: special contact algorithm to handle sheet blank edge (deformable) to gage pin (rigid shell) contact during implicit gravity loading, applies to *CONTACT_FORM- ING_NODES_TO_SURFACE only. See more details in About SOFT = 6. The soft constraint may be necessary if the material constants of the elements which make up the surfaces in contact have a wide variation in the elastic bulk moduli. In the soft constraint option, the interface stiffness is based on the nodal mass and the global time step size. This method of computing the interface stiffness will typically give much higher stiffness value than would be obtained by using the bulk modulus; therefore, this method the preferred approach when soft foam materials interact with metals. See the remark below for the segment-based penalty formulation. SOFSCL LCIDAB MAXPAR *CONTACT_OPTION1_{OPTION2}_… DESCRIPTION Scale factor for constraint forces of soft constraint option (default=.10). Values greater than .5 for single surface contact and 1.0 for a one-way treatment are inadmissible. Load curve ID defining airbag thickness as a function of time for type a13 contact (*CONTACT_AIRBAG_SINGLE_SURFACE). Maximum parametric coordinate in segment search (values between 1.025 and 1.20 are recommended). This variable applies only to SMP; for MPP, see PARMAX. Larger values can increase cost. If zero, the default is set to 1.025 for most contact options. Other defaults are: EQ.1.006: SPOTWELD, EQ.1.006: TIED_SHELL_…_CONSTRAINED_OFFSET, EQ.1.006: TIED_SHELL_…_OFFSET, EQ.1.006: TIED_SHELL_…_:BEAM_OFFSET, EQ.1.100: AUTOMATIC_GENERAL This factor allows an increase in the size of the segments which may be useful at sharp corners. For the SPOTWELD and …_ OFFSET options larger values can sometimes lead to numerical instabilities; however, a larger value is sometimes necessary to ensure that all nodes of interest are tied. SBOPT Segment-based contact options (SOFT = 2). EQ.0: defaults to 2. EQ.1: pinball edge-edge contact (not recommended) EQ.2: assume planer segments (default) EQ.3: warped segment checking EQ.4: sliding option EQ.5: do options 3 and 4 VARIABLE DEPTH BSORT FRCFRQ DESCRIPTION Search depth in automatic contact, check for nodal penetration through the closest contact segments. Value of 1 (one segment) is sufficiently accurate for most crash applications and is much less expensive. LS-DYNA for improved accuracy sets this value to 2 (two segments), which is default when set to zero, default search depth for *CONTACT_AUTOMATIC_GENERAL is 3. LT.0: |DEPTH| is the load curve ID defining searching depth versus time. (not available when SOFT = 2) See remarks below for segment-based contact (SOFT = 2) options controlled by DEPTH. Number of cycles between bucket sorts. Values of 25 and 100 are recommended for contact types 4 and 13 (SINGLE_SURFACE), respectively. Values of 10-15 are okay for the surface to surface and node to surface contact. If zero, LS-DYNA determines the interval. BSORT applies only to SMP except in the case of SOFT = 2 or for Mortar contact (option MORTAR on the CONTACT card), in which case BSORT applies to both SMP and MPP. For Mortar contact the default is the value associated with NSBCS on *CONTROL_CONTACT. LT.0: |BSORT| load curve ID defining bucket sorting frequency versus time. Number of cycles between contact force updates for penalty contact formulations. This option can provide a significant speed-up of the contact treatment. If used, values exceeding 3 or 4 are dangerous. Considerable care must be exercised when using this option, as this option assumes that contact does not change FRCFRG cycles. EQ.0: FRCFRG is set to 1 and force calculations are performed each cycle-strongly recommended. Nodes in NSET #21 (create 'by path' in LSPP4.0) Sheet blank Sheet blank Fixed in XZ Gage pin (PID 20) Fixed in Z Fixed in XZ Gravity loading in -Y Gage pin Binder ring Lower post Figure 11-11. Illustrative/test model for SOFT = 6 (left) and initial blank position. General remarks: Setting SOFT = 1 or 2 on optional contact card A will cause the contact stiffness to be determined based on stability considerations, taking into account the time step and nodal masses. This approach is generally more effective for contact between materials of dissimilar stiffness or dissimilar mesh densities. About SOFT = 2: SOFT = 2 is for general shell and solid element contact. This option is available for SURFACE_TO_SURFACE, ONE_WAY_SURFACE_TO_SURFACE, and SINGLE_SUR- FACE options including AUTOMATIC, ERODING, and AIRBAG contact. When the AUTOMATIC option is used, orientation of shell segment normals is automatic. When the AUTOMATIC option is not used, the segment or element orientations are used as input. The segment-based penalty formulation contact algorithm checks for segments vs. segment penetration rather than node vs. segment. After penetrating segments are found, an automatic judgment is made as to which is the master segment, and penalty forces are applied normal to that segment. The user may override this automatic judgment by using the ONE_WAY options in which case the master segment normals are used as input by the user. All parameters on the first three cards are active except for VC, and VSF. On optional card A, some parameters have different meanings than they do for the default contact. For SOFT = 2, the SBOPT parameter on optional card A controls several options. Setting DEPTH = 1 for pinball edge-to-edge checking is not recommended and is included only for back compatibility. For edge-to-edge checking setting DEPTH = 5 is recommended instead . The warped segment option more accurately checks for penetration of warped surfaces. The sliding option uses neighbor segment information to improve sliding behavior. It is primarily useful for preventing segments from incorrectly catching nodes on a sliding surface. For SOFT = 2, the DEPTH parameter controls several additional options for segment based contact. 1. DEPTH = 2 (former default; not recommended). surface penetrations measured at nodes are checked. 2. DEPTH = 3 (current default). Surface penetration is also be measured at the edge. This option is more accurate than DEPTH=2, and is good for a wide variety of simulations, but does not check for edge-to-edge penetration. 3. DEPTH = 5. Both surface penetrations and edge-to-edge penetration is checked. 4. DEPTH = 13. The penetration checking is the same as for DEPTH=3, but the code has been tuned to better conserve energy. 5. DEPTH = 23 or 33. The penetration checking is similar to DEPTH=3, but new methods are used to try to improve robustness. 6. DEPTH = 25 or 35. The penetration checking is similar to DEPTH=5 but use new methods to try to improve robustness. 7. DEPTH = 45. The splitting pinball method [Belytschko and Yeh, 1993] is used. This method is more accurate at the cost of more CPU time, and is recommend- ed when modeling complex contacts between parts comprised of shells. It does not apply to solid or thick shell parts but such parts can be coated with null shells as a means of making DEPTH=45 available. 8. DEPTH = 1 or 4. The airbag contact has two additional options, DEPTH=1 and 4. DEPTH=4 activates additional airbag logic that uses neighbor segment in- formation when judging if contact is between interior or exterior airbag surfac- es. This option is not recommended and is maintained only for backward compatibility. Setting DEPTH=1 suppresses all airbag logic. For SOFT = 2 contact, only the ISYM, I2D3D, SLDTHK, and SLDSTF parameters are active on optional card B. Also, the negative MAXPAR option is now incorporated into the DTSTIF option on optional card C. Data that uses the negative MAXPAR option will continue to run correctly. Binder ring Pin / blank edge contact enforced Lower post Gage pin Sheet blank final position Sheet blank final position Gravity loading results without using SOFT=6; Pin/blank edge contact missed. Gravity loading results using SOFT=6; Pin/blank edge contact sucessful. Figure 11-12. Final blank position without (left) and with (right) SOFT = 6. About SOFT = 6: SOFT = 6 contact addresses contact issues in situation where blank gage pins are narrow or small and blank mesh are coarse (Figure 11-11 left), leading to missing contact in some cases. This feature applies only to gravity loading of sheet blank with non-adaptive mesh, and for use with *CONTACT_FORMING_NODES_TO_SUR- FACE only. set for included in a node the variable SSID Nodes along the entire or a portion of the blank edge to be contacted with gage pins * CON- must be TACT_FORMING_NODES_TO_SURFACE (Figure 11-11 left). The nodes in the node set must be listed in a consecutive order, as defined “by path” in LSPP4.0, under Model → CreEnt → Cre → Set Data → *SET_NODE. No thickness exists for either blank edge or gage pins. In addition, the variable ORIENT in *CONTROL_CONTACT must be set to “4”. Currently this feature is available in double precision, SMP only, starting in in Revision 81297 and *CONTACT_FORMING_NODES_TO_SURFACE can be input as part ID of the blank, making it much easier to use SOFT = 6. in Revision 110072, SSID later releases. Starting in In a partial keyword example below, node set ID 21 (SSTYP = 4) is in contact with gage pin of part set ID 20. As shown in Figure 11-11 (left), with the boundary condition applied, a blank with a very coarse mesh is loaded with a body force. The left notch is anticipated to be in contact with the gage pins. The initial position (top view) of the test model is shown in Figure 11-11 (right) and the final gravity loaded blank positions are shown in Figure 11-12 (left) without SOFT = 6, and in Figure 11-12 (middle and right) with SOFT = 6, respectively. It is shown that without the SOFT = 6 the contact between the blank edge and the pin missed completely. *CONTROL_TERMINATION 1.0 *CONTROL_IMPLICIT_FORMING 1 *CONTROL_IMPLICIT_GENERAL 1,0.2 *CONTROL_IMPLICIT_NONLINEAR $ NSLOLVR ILIMIT MAXREF DCTOL ECTOL RCTOL LSTOL 2 1 1200 0.000 0.00 0 $ dnorm divflag inistif 0 2 0 1 1 *SET_NODE_LIST $ blank edge node set around the gage pin 21 1341,1342,1343,1344 *SET_PART_LIST $ gage pin 20 20 *SET_PART_LIST $ blank 13 13 *CONTACT_FORMING_NODES_TO_SURFACE $ SSID MSID SSTYP MSTYP SBOXID MBOXID SPR MPR 21 20 4 2 $ FS FD DC V VDC PENCHK BT DT 0.125 20. 4 $ SFS SFM SST MST SFST SFMT FSF VSF $ SOFT 6 Beginning in Revision109342, an SSTYP of 3 (a part PID, not a part set ID) can be used for the SSID, simplifying the definition of contact interfaces for SOFT = 6. In Soft 6 contact definition below, a blank PID of 13 is defined for the SSID using SSTYP = 3: *CONTACT_FORMING_NODES_TO_SURFACE $ SSID MSID SSTYP MSTYP SBOXID MBOXID SPR MPR 13 20 3 2 $ FS FD DC V VDC PENCHK BT DT 0.125 20. 4 $ SFS SFM SST MST SFST SFMT FSF VSF $ SOFT 6 Optional Card B: Reminder: If Optional Card B is used, then Optional Card A must be defined. (Optional Card A may be a blank line). Optional Card B. Optional 1 2 3 4 5 6 7 8 Variable PENMAX THKOPT SHLTHK SNLOG ISYM I2D3D SLDTHK SLDSTF Type Default F 0 I 0 I 0 I 0 I 0 I 0 F 0 F 0 Remarks VARIABLE PENMAX Old types 3, 5, 10 Old types 3, 5, 10 DESCRIPTION Maximum penetration distance for old type 3, 5, 8, 9, 10 and Mortar contact or the segment thickness multiplied by PENMAX defines the maximum penetration allowed (as a multiple of the segment thickness) for contact types a 3, a 5, a10, 13, 15, and 26. : EQ.0.0: for old type contacts 3, 5, and 10: Use small penetration search and value calculated from thickness and XPENE, see *CONTROL_CONTACT. EQ.0.0: for contact types a 3, a 5, a10, 13, and 15: Default is 0.4, or 40 percent of the segment thickness EQ.0.0: for contact type26 the default value is the segment thickness multiplied by 10 EQ.0.0: for Mortar contact the default is a characteristic size of the element, see Theory manual VARIABLE DESCRIPTION THKOPT Thickness option for contact types 3, 5, and 10: SHLTHK EQ.0: default is taken from control card, *CONTROL_CON- TACT, EQ.1: thickness offsets are included, EQ.2: thickness offsets are not included (old way). Define if and only if THKOPT above equals 1. Shell thickness considered in type surface to surface and node to surface type contact options, where options 1 and 2 below activate the new contact algorithms. The thickness offsets are always included in single surface and constraint method contact types: EQ.0: thickness is not considered, EQ.1: thickness is considered but rigid bodies are excluded, EQ.2: thickness is considered including rigid bodies. SNLOG Disable shooting node logic in thickness offset contact. With the shooting node logic enabled, the first cycle that a slave node penetrates a master segment, that node is moved back to the master surface without applying any contact force. EQ.0: logic is enabled (default), EQ.1: logic is skipped for (sometimes metalforming calculations or for contact involving foam materials). recommended ISYM Symmetry plane option: EQ.0: off, EQ.1: do not include faces with normal boundary constraints (e.g., segments of brick elements on a symmetry plane). This option is important to retain the correct boundary conditions in the model with symmetry. For the ERODING contacts this option may also be defined on card 4. I2D3D Segment searching option: EQ.0: search 2D elements (shells) before 3D elements (solids, thick shells) when locating segments. EQ.1: search 3D (solids, thick shells) elements before 2D elements (shells) when locating segments. VARIABLE SLDTHK SLDSTF DESCRIPTION Optional solid element thickness. A nonzero positive value will activate the contact thickness offsets in the contact algorithms The contact treatment will then be where offsets apply. equivalent to the case where null shell elements are used to cover the brick elements. The contact stiffness parameter below, SLDSTF, may also be used to override the default value. This parameter applies also to Mortar contacts, but SLDSTF is then ignored. Optional solid element stiffness. A nonzero positive value overrides the bulk modulus taken from the material model referenced by the solid element. For segment based contact (SOFT = 2), SLDSTF replaces the stiffness used in the penalty equation. This parameter does not apply to Mortar contacts. *CONTACT_OPTION1_{OPTION2}_… Reminder: If Optional Card C is used, then Optional Cards A and B must be defined. (Optional Cards A and B may be blank lines). Optional Card C. Optional 1 2 3 4 5 6 7 8 Variable IGAP IGNORE DPRFAC / MPAR1 DTSTIF / MPAR2 FLANGL CID_RCF Type Default I 1 Remarks VARIABLE IGAP I 0 3 F 0 1 F 0 2 F 0 I 0 DESCRIPTION For mortar contact IGAP is used to progressively increase contact stiffness for large penetrations, see remarks on mortar contact below. For other contacts it is a flag to improve implicit convergence behavior at the expense of (1) creating some sticking if parts attempt to separate and (2) possibly underreporting the contact force magnitude in the output files rcforc and ncforc. (IMPLICIT ONLY.). LT.0: Set IGAP = 1 and set the distance for turning on the stiffness to (IGAP/10) times the original distance. EQ.1: Apply method to improve convergence (DEFAULT) EQ.2: Do not apply method GT.2: Set IGAP = 1 for first IGAP − 2 converged equilibrium states, then set IGAP = 2 VARIABLE IGNORE Ignore options. DESCRIPTION initial penetrations in the *CONTACT_AUTOMATIC LT.0: Applies only to the Mortar contact. When less than zero, the behavior is the same as for |IGNORE|, but contact be- tween segments belonging to the same part is ignored. The main purpose of this option is to avoid spurious contact detections that otherwise could result for compli- cated geometries in a single surface contact, typically, when eliminating initial penetrations by interference. See IGNORE.EQ.3 and IGNORE.EQ.4. EQ.0: Take the default value from the fourth card of the CON- TROL_CONTACT input. EQ.1: Allow initial penetrations to exist by tracking the initial penetrations. EQ.2: Allow initial penetrations to exist by tracking the initial penetrations. However, penetration warning messages are printed with the original coordinates and the recommend- ed coordinates of each slave node given. EQ.3: Applies only to the Mortar contact. With this option initial penetrations are eliminated between time zero and the time specified by MPAR1. Intended for small initial pene- trations. See remarks on Mortar contact. EQ.4: Applies only to the Mortar contact. With this option initial penetrations are eliminated between time zero and the time specified by MPAR1. In addition a maximum pene- tration distance can be given as MPAR2, intended for large initial penetrations. See remarks on Mortar contact. VARIABLE DPRFAC/ MPAR1 DESCRIPTION Applies to the SOFT = 2 and Mortar contacts. Depth of penetration reduction factor (DPRFAC) for SOFT = 2 contact. EQ.0.0: Initial penetrations are always ignored. GT.0.0: Initial penetrations are penalized over time. LE.-1.0: |DPRFAC| is the load curve ID defining DPRFAC versus time. For the mortar contact MPAR1 corresponds to initial contact pressure in interfaces with initial penetrations if IGNORE = 2, for IGNORE = 3,4 it corresponds to the time of closure of initial penetrations. See remarks below. DTSTIF/ MPAR2 Applies to the SOFT = 1 and SOFT = 2 and Mortar contacts. Time step used in stiffness calculation for SOFT = 1 and SOFT = 2 contact. EQ.0.0: Use the initial value that is used for time integration. GT.0.0: Use the value specified. ∈ (−1.0, −0.01): use a moving average of the solution time step. (SOFT = 2 only) LE.-1.0: |DTSTIF| is the ID of a curve that defines DTSTIF vs. time. For the mortar contact and IGNORE = 4, MPAR2 corresponds a penetration depth that must be at least the penetration occurring in the contact interface. See remarks below. FLANGL Angle tolerance in radians for feature lines option in smooth contact. EQ.0.0: No feature line is considered for surface fitting in smooth contact. GT.0.0: Any edge with angle between two contact segments bigger than this angle will be treated as feature line dur- ing surface fitting in smooth contact. CID_RCF Coordinate system ID to output rcforc force resultants and ncforc data in a local system. Remarks: 1. DPRFAC/MPAR1 is used only by segment based contact (SOFT = 2) and Mortar Contact . By default, SOFT = 2 contact measures the initial penetration between segment pairs that are found to be in contact and subtracts the measured value from the total pene- tration for as long as a pair of segments remains in contact. The penalty force is proportional to this modified value. This approach prevents shooting nodes, but may allow unacceptable penetration. DPRFAC can be used to decrease the measured value over time until the full penetration is penalized. Setting DPR- FAC = 0.01 will cause ~1% reduction in the measured value each cycle. The maximum allowable value for DPRFAC is 0.1. A small value such as 0.001 is recommended. DPRFAC does not apply to initial penetrations at the start of the calculation, only those that are measured at later times. This prevents non- physical movement and energy growth at the start of the calculation. 2. The anticipated use for the load curve option is to allow the initial penetrations to be reduced at the end of a calculation if the final geometry is to be used for a subsequent analysis. To achieve this, load curve should have a y-value of zero until a time near the end of the analysis and then ramp up to a positive value such as 0.01 near the end of the analysis. 3. DTSTIF/MPAR2 is used only by the SOFT = 1 and SOFT = 2 contact options and the Mortar contact (for the latter, see remarks on Mortar contact). By de- fault when the SOFT option is active, the contact uses the initial solution time step to scale the contact stiffness. If the user sets DTSTIF to a nonzero value, the inputted value will be used. Because the square of the time step appears in the denominator of the stiffness calculation, a DTSTIF value larger than the initial solution time step reduces the contact stiffness and a smaller value increases the stiffness. This option could be used when one component of a larger model has been analyzed independently and validated. When the component is inserted into the larger model, the larger model may run at a smaller time step due to higher mesh frequencies. In the full model analysis, setting DTSTIF equal to the component analysis time step for the contact interface that treats the component will cause consistent contact stiffness between the analyses. The load curve option allows contact stiffness to be a function of time. This should be done with care as energy will not be conserved. A special case of the load curve option is when |DTSTIF| = LCTM on *CONTROL_CONTACT. LCTM sets an upper bound on the solution time step. For |DTSTIF| = LCTM, the contact stiffness time step value will track LCTM whenever the LCTM value is less than the initial solution time step. If the LCTM value is greater, the initial solution time step is used. This option could be used to stiffen the contact at the end of an analysis. To achieve this, the LCTM curve should be defined such that it is larger than the solution time step until near the end of the analysis. Then the LCTM curve should ramp down below the solution time step causing it to decrease and the contact to stiffen. A load curve value of 0.1 of the calcu- lated solution time step will cause penetrations to reduce by about 99%. To prevent shooting nodes, the rate at which the contact stiffness increases is au- tomatically limited. Therefore, to achieve 99% reduction, the solution should be run for perhaps 1000 cycles with a small time step. For segment based contact (SOFT = 2), setting DTSTIF less than or equal to -0.01 and greater than -1.0, causes the contact stiffness to be updated based on the current solution time step. Varying the contact stiffness during a simulation can cause energy growth so this option should be used with care when extra stiffness is needed to prevent penetration and the solution time step has dropped from the initial. Because quick changes in contact stiffness can cause shooting nodes, using a moving average of the solution time step can prevent this. The value of DTSTIF determines the number of terms in the moving aver- age where n = 100 × (-DTSTIF) such that n = 1 for DTSTIF = -0.01 and n = 100 for DTSTIF = -0.999. Setting DTSTIF = -1.0 triggers the load curve option de- scribed in the previous paragraph, so DTSTIF cannot be smaller than -0.999 for this option. 4. When SOFT = 2 on Optional Card A of *CONTACT, treatment of initial penetrations is always like IGNORE = 1 in that initial penetrations are ignored when calculating penalty forces. If SOFT = 2 and IGNORE = 2, then a report of initial penetrations will be written to the messag file(s) in the first cycle. Optional Card D: Reminder: If Optional Card D is used, then Optional Cards A, B and C must be defined. (Optional Cards A, B and C may be blank lines). Optional Card D. Optional 1 2 3 4 5 6 7 8 Variable Q2TRI DTPCHK SFNBR FNLSCL DNLSCL TCSO TIEDID SHLEDG Type Default Remarks I 0 1 VARIABLE Q2TRI F 0 2 F 0 3 F 0 5 F 0 5 I 0 I 0 4 I DESCRIPTION Option to split quadrilateral contact segments into two triangles (only available when SOFT = 2). EQ.0: Off (default). EQ.1: On for all slave shell segments. EQ.2: On for all master shell segments. EQ.3: On for all shell segments. EQ.4: On for all shell segments of material type 34. DTPCHK Time interval between shell penetration reports (only available for segment based contact) EQ.0.0: Off (default). GT.0.0: Check and report segment penetrations at time intervals equal to DTPCHK SFNBR *CONTACT_OPTION1_{OPTION2}_… DESCRIPTION Scale factor for neighbor segment contact (only available for segment based contact) EQ.0.0: Off (default). GT.0.0: Check neighbor segments for contact LT.0.0: Neighbor segment checking with improved energy balance when |SFNBR| < 1000. |SFNBR|≥1000 acti- vates a split-pinball based neighbor contact with a pen- alty force scale factor of |SFNBR+1000|. For example, force scale factor used is 2 when SFNBR = -1002. FNLSCL Scale factor for nonlinear force scaling. TCSO Option to consider only contact segments (not all attached elements) when computing the contact thickness for a node or (for SEGMENT_TO_SEGMENT contact and shell segment elements only) EQ.0: Off (default). EQ.1: Only consider segments in the contact definition DNLSCL Distance for nonlinear force scaling. TIEDID Incremental displacement update for tied contacts. EQ.0: Off (default). EQ.1: On SHLEDG Flag for assuming edge shape for shells when measuring penetration. This is available for segment based contact EQ.0: default to SHLEDG on *CONTROL_CONTACT EQ.1: Shell edges are assumed square and are flush with the nodes EQ.2: Shell edges are assumed round with radius equal to ½ shell thickness Remarks: 1. Q2TRI. Setting Q2TRI to a nonzero value causes quadrilateral shell segments to be spilt into two triangles. The contact segments only are split. The elements are not changed. This option is only available for segment based contact which is activated by setting SOFT = 2. 2. DTPCHK (Penetration Check). Setting DTPCHK to a positive value causes a penetration check to be done periodically with the interval equal to DTPCHK. The check looks for shell segments that are penetrating the mid-plane of anoth- er shell segment. It does not report on penetration of thickness offsets. The penetrating pairs are reported to the messag file or files for MPP. If at least one penetration is found, the total number of pairs is reported to the screen output. This option is only available for segment based contact which is activated by setting SOFT = 2. 3. SFNBR. SFNBR is a scale factor for optional neighbor segment contact checking. This is available only in segment based (SOFT=2) contact. This is helpful option when a mesh folds as can happen with compression folding of an airbag. Only shell element segments are checked. Setting SFNBR to a nega- tive value modifies the neighbor checking to improve energy balance. When used, a value between -0.5 and -1.0 is recommended. 4. Round off in OFFSET and TIEBREAK. There have been several issues with tied OFFSET contacts and AUTOMATIC_TIEBREAK contacts with offsets creat- ing numerical round-off noise in stationary parts. By computing the interface displacements incrementally rather than using total displacements, the round- off errors that occur in single precision are eliminated. The incremental ap- proach is available for the following contact types: TIED_SURFACE_TO_SURFACE_OFFSET TIED_NODES_TO_SURFACE_OFFSET TIED_NODES_TO_SURFACE_CONSTRAINED_OFFSET TIED_SHELL_EDGE_TO_SURFACE_OFFSET AUTOMATIC_…_TIEBREAK 5. FNLSCL. FNLSCL = 𝑓 and DNLSCL = 𝑑 invoke alternative contact stiffness scaling options. When FNLSCL > 0 and DNLSCL > 0, the first option scales the stiffness by the depth of penetration to provide smoother initial contact and a larger contact force as the depth of penetration exceeds DNLSCL. The stiffness k is scaled by the relation 𝑘 → 𝑘𝑓 √ where 𝛿 is the depth of penetration, making the penalty force proportional to the 3/2 power of the penetration depth. Adding a small amount of surface damping (e.g., VDC = 10) is advised with this option. When SOFT = 2 and FNLSCL < 0, DNLSCL > 0, an alternative stiffness scaling scheme is used, 𝑘 → 𝑘 [ 0.01𝑓 𝐴𝑜 𝑑(𝑑 − 𝛿) ] where 𝐴0 is the overlap area of segments in contact. For 𝛿 greater than 0.9𝑑, the stiffness is extrapolated to prevent it from going to infinity. When SOFT = 2, FNLSCL > 0, and DNLSCL = 0, an option to scale the contact by the overlap area is invoked. 𝑘 → 𝑘𝑓 ( 𝐴𝑜 𝐴𝑚 ) where 𝐴𝑚 is the mean area of all the contact segments in the contact interface. This third option can improve friction behavior, particularly when the FS = 2 option is used. Optional Card E: Reminder: If Optional Card E is used, then Optional Cards A, B, C and D must be defined. (Optional Cards A, B, C and D may be blank lines). Optional Card E. Optional 1 2 3 4 5 6 7 8 Variable SHAREC CPARM8 IPBACK SRNDE FRICSF ICOR FTORQ REGION Type Default Remarks I 0 1 I 0 I 0 2 I 0 3 F 1. 5 I 0 I 0 I 0 4 VARIABLE DESCRIPTION SHAREC Shared constraint flag (only available for segment based contact) CPARM8 EQ.0: Segments that share constraints not checked for contact. EQ.1: Segments that share constraints are checked for contact. This variable is similar to CPARM8 in *CONTACT_…_MPP but applies to SMP and not to MPP. CPARM8 for SMP only controls treatment of spot weld beams in CONTACT_AUTOMATIC_- GENERAL. EQ.0: Spot weld (type 9) beams are not considered in the contact even if included on the slave side of the contact. EQ.2: Spot weld (type 9) beams are considered in the contact if included on the slave side of the contact. IPBACK If set to a nonzero value, creates a “backup” penalty tied contact for this interface. This option applies to constrained tied contacts only. See Remark 2. SRNDE *CONTACT_OPTION1_{OPTION2}_… DESCRIPTION Flag for non-extended exterior shell edges. See Remark 3 below for further information and restrictions: EQ.0: Exterior shell edges have their usual treatment where the contact surface extends beyond the shell edge. EQ.1: The contact surface is rounded at exterior shell edges but does not extend beyond the shell edges. EQ.2: The shell edges are square. FRICSF Scale factor for frictional stiffness (available for SOFT = 2 only). ICOR FTORQ If set to a nonzero value, VDC is the coefficient of restitution expressed as a percentage. When SOFT = 0 or 1, this option applies to AUTOMATIC_NODES_TO_SURFACE, AUTOMAT- IC_SURFACE_TO_SURFACE and AUTOMATIC_SINGLE_SUR- FACE. When SOFT = 2, it applies to all available keywords. If set to 1, a torsional force is computed in the beam to beam portion of contact type AUTOMATIC_GENERAL, which balances the torque produced due to friction. This is currently only available in the MPP version. REGION The ID of a *DEFINE_REGION which will delimit the volume of space where this contact is active. See Remark 4 below. Remarks: 1. The SHAREC flag is a segment based contact option that allows contact checking of segment pairs that share a multi-point constraint or rigid body. Sharing a constraint is defined as having at least one node of each segment that belongs to the same constraint. 2. The IPBACK flag is only applicable to constraint based tied contacts (TIED with no options, or with CONSTRAINED_OFFSET). An identical penalty based contact is generated with type OFFSET, except in the case of SHELL_EDGE constrained contact which generates a BEAM_OFFSET type. The ID of the generated interface will be set to the ID of the original interface plus 1 if that ID is available, otherwise one more than the maximum used contact ID. For nodes successfully tied by the constraint interface, the extra penalty tying should not cause problems, but nodes dropped from the constraint interface due to rigid body or other conflicting constraints will be handled by the penalty contact. In MPP, nodes successfully tied by the constraint interface are skipped during the penalty contact phase. 3. The SRNDE option only applies to SOFT = 0 and SOFT = 1 contacts in the MPP version. Shell edges for these contacts are by default treated by adding cylin- drical caps along the free edges, with the radius of the cylinder equal to half the thickness of the segment. This has the side effect of extending the segment at the free edges, which can cause problems. Setting SRNDE = 1 “rounds over” the (through the thickness) corners of the element instead of extending it. The edges of the segment are still rounded, but the overall size of the contact area is not increased. The effect is as if the free edge of the segment was moved in toward the segment by a distance equal to half the segment thickness, and then the old cylindrical treatment was performed. Setting SRNDE = 2 will treat the shell edges as square, with no extension. This variable has no effect on shell- edge-to-shell-edge interaction in AUTOMATIC_GENERAL; for that, see CPAR- M8 on the MPP Card. The SRNDE = 1 option is available for the AUTOMATIC_SINGLE and AUTO- MATIC_GENERAL contacts. The NODE_TO_SURFACE and SURFACE_TO_- SURFACE contacts also support SRNDE = 1 if the GROUPABLE option is used. The SRNDE = 2 option is available for all these contact types if the GROUPA- BLE option is enabled. 4. Setting a non-zero value for REGION does not limit or in any way alter the list of slave or master nodes or segments, and this option should not be used for that purpose. For efficiency, the smallest possible portion of the model should be defined as slave or master using the normal mechanisms for specifying the slave and master surfaces. Setting a non-zero value will, however, result in contact outside the REGION being ignored. As slave and master nodes and segments pass into the indicated REGION, contact for them will become active. As they pass out of the REGION, they will be skipped in the contact calculation. This option is currently only available for the MPP version, and only for con- tacts of type AUTOMATIC_SINGLE_SURFACE, and AUTOMATIC_*_TO_- SURFACE. 5. The FRICSF factor is an optional factor to scale the frictional stiffness. FRICSF is available only when SOFT = 2 on optional card A. With penalty contact, the frictional force is a function of the stiffness, the sliding distance, and the Cou- lomb limit. *CONTACT_OPTION1_{OPTION2}_… Reminder: If Optional Card F is used, then Optional Cards A, B, C, D and E must be defined. (Optional Cards A, B, C, D and E may be blank lines). Optional Card F. Optional 1 2 3 4 5 6 7 8 Variable PSTIFF IGNROFF Type Default Remarks I 0 1 VARIABLE PSTIFF I 0 DESCRIPTION Flag to choose the method for calculating the penalty stiffness. This is available for segment based contact EQ.0: Use the default as defined by PSTIFF on *CONTROL_- CONTACT. EQ.1: Based on nodal masses EQ.2: Based on material density and segment dimensions. IGNROFF Flag to ignore the thickness offset for shells in the calculation of the shell contact penetration depth. This allows shells to be used for meshing rigid body dies without modifying the positions of the nodes to compensate for the shell thickness. EQ.1: Ignore the master side thickness. EQ.2: Ignore the slave side thickness. EQ.3: Ignore the thickness of both sides.. Remarks: 1. See Remark 6 on *CONTROL_CONTACT for an explanation of the PSTIFF option. Specifying PSTIFF here will override the default value as defined by PSTIFF on *CONTROL_CONTACT. General Remarks: *CONTACT 1. Modeling airbag interactions with structures and occupants using the actual fabric thickness, which is approximate 0.30 mm, may result in a contact break- down that leads to inconsistent occupant behavior between different machines. Based on our experience, using a two-way automatic type contact definition, i.e., AUTOMATIC_SURFACE_TO_SURFACE, between any airbag to struc- ture/occupant interaction and setting the airbag fabric contact thickness to at least 10 times the actual fabric thickness has helped improved contact behavior and eliminates the machine inconsistencies. Due to a large stiffness difference between the airbag and the interacting materials, the soft constraint option (SOFT = 1) or the segment based option (SOFT = 2) is recommended. It must be noted that with the above contact definition, only the airbag materials should be included in any *AIRBAG_SINGLE_SURFACE definitions to avoid duplicate contact treatment that can lead to numerical instabilities. 2. The following contact definitions are based on constraint equations and will not work with rigid bodies: TIED_NODES_TO_SURFACE TIED_NODES_TO_SURFACE_CONSTRAINED_OFFSET TIED_SURFACE_TO_SURFACE TIED_SURFACE_TO_SURFACE_CONSTRAINED_OFFSET TIED_SHELL_EDGE_TO_SURFACE TIED_SHELL_EDGE_TO_SURFACE_CONSTRAINED_OFFSET TIED_SHELL_EDGE_TO_SOLID SPOTWELD SPOTWELD_WITH_TORSION However, SPOTWELD_WITH_TORSION_PENALTY does work with rigid bodies and tied interfaces with the offset option can be used with rigid bodies, i.e., TIED_NODES_TO_SURFACE_OFFSET TIED_SHELL_EDGE_TO_SURFACE_OFFSET TIED_SHELL_EDGE_TO_SURFACE_BEAM_OFFSET TIED_SURFACE_TO_SURFACE_OFFSET Also, it may sometimes be advantageous to use the CONSTRAINED_EXTRA_- NODE_OPTION instead for tying deformable nodes to rigid bodies since in this latter case the tied nodes may be an arbitrary distance away from the rigid body. Tying will only work if the surfaces are near each other. The criteria used to determine whether a slave node is tied down is that it must be “close”. For shell elements “close” is defined as distance, 𝛿, less than: 𝛿1 = 0.60 × (thickness of slave node + thickness of master segment) 𝛿2 = 0.05 × min(master segment diagonals) 𝛿 = max(𝛿1, 𝛿2) If a node is further away it will not be tied and a warning message will be printed. For solid elements the slave node thickness is zero and the segment thickness is the element volume divided by the segment area; otherwise, the same procedure is used. If there is a large difference in element areas between the master and slave side, the distance, 𝛿2, may be too large and may cause the unexpected projection of nodes that should not be tied. This can occur during calculation when adaptive remeshing is used. To avoid this difficulty the slave and master thickness can be specified as negative values on Card 3 in which case 𝛿 = abs(𝛿1) 3. The contact algorithm for tying spot welds with torsion, SPOTWELD_WITH_- TORSION, must be used with care. Parts that are tied by this option should be subjected to stiffness proportional damping of approximately ten percent, i.e., input a coefficient of 0.10. This can be defined for each part on the *DAMP- ING_PART_STIFFNESS input. Stability problems may arise with this option if damping is not used. This comment applies also to the PENALTY keyword option. 4. These contact definitions must be used with care. The surface and the nodes which are constrained to a surface are not allowed to be used in any other CONSTRAINT_… contact definition: CONSTRAINT_NODES_TO_SURFACE CONSTRAINT_SURFACE_TO_SURFACE If, however, contact has to be defined from both sides as in sheet metal forming, one of these contact definitions can be a CONSTRAINT type; the other one could be a standard penalty type such as SURFACE_TO_SURFACE or NODES_TO_SURFACE. 5. These contact definitions require thickness to be taken into account for rigid bodies modeled with shell elements. Therefore, care should be taken to ensure that realistic thicknesses are specified for the rigid body shells. AIRBAG_SINGLE_SURFACE AUTOMATIC_GENERAL AUTOMATIC_GENERAL_INTERIOR AUTOMATIC_NODES_TO_SURFACE AUTOMATIC_ONE_WAY_SURFACE_TO_SURFACE AUTOMATIC_SINGLE_SURFACE AUTOMATIC_SURFACE_TO_SURFACE SINGLE_SURFACE A thickness that is too small may result in loss of contact and an unrealistically large thickness may result in a degradation in speed during the bucket sorts as well as nonphysical behavior. The SHLTHK option on the *CONTROL_CON- TACT card is ignored for these contact types. 6. Two methods are used in LS-DYNA for projecting the contact surface to account for shell thicknesses. The choice of methods can influence the accuracy and cost of the calculation. Segment based projection is used in contact types: AIRBAG_SINGLE_SURFACE AUTOMATIC_GENERAL AUTOMATIC_NODES_TO_SURFACE AUTOMATIC_ONE_WAY_SURFACE_TO_SURFACE AUTOMATIC_SINGLE_SURFACE AUTOMATIC_SURFACE_TO_SURFACE Nodal normal projection Segment based projection Figure 11-13. Nodal normal and segment based projection is used in the contact options FORMING_NODES_TO_SURFACE FORMING_ONE_WAY_SURFACE_TO_SURFACE FORMING_SURFACE_TO_SURFACE The remaining contact types use nodal normal projections if projections are used. The main advantage of nodal projections is that a continuous contact surface is obtained which is much more accurate in applications such as metal forming. The disadvantages of nodal projections are the higher costs due to the nodal normal calculations, difficulties in treating T-intersections and other geometric complications, and the need for consistent orientation of contact surface segments. The contact type SINGLE_SURFACE uses nodal normal projections and consequently is slower than the alternatives. 7. These contact algorithms allow the total contact forces applied by all contacts to be picked up. FORCE_TRANSDUCER_PENALTY FORCE_TRANSDUCER_CONSTRAINT 8. This contact does not apply any force to the model and will have no effect on the solution. Only the slave set and slave set type need be defined for this con- tact type. Generally, only the first three cards are defined. The force transducer option, PENALTY, works with penalty type contact algorithms only, i.e., it does Contact surface augment SLDTHK Contact surface augment (SST × SFST-T)/2 Element thickness T Figure 11-14. Illustration of contact surface location for automatic Mortar contact, solids on top and shells below. not work with the CONSTRAINT or TIED options. For these latter options, use the CONSTRAINT option. If a transducer is used for extracting forces from Mortar contacts, the slave and master sides must be defined through parts or part sets, segment or node sets will not gather the correct data. NOTE: If the interactions between two surfaces are needed, a master surface should be defined. In this case, only the contact forces applied between the slave and master surfaces are kept. The master surface option is only implemented for the PENALTY option and works only with the AUTOMATIC contact types. 9. FORMING_… These contacts are mainly used for metal forming applications. A connected mesh is not required for the master (tooling) side but the orienta- tion of the mesh must be in the same direction. These contact types are based on the AUTOMATIC type contacts and consequently the performance is better than the original two surface contacts. 10. The mortar contact, invoked by appending the suffix MORTAR to either FORMING_SURFACE_TO_SURFACE, AUTOMATIC_SURFACE_TO_SUR- FACE or AUTOMATIC_SINGLE_SURFACE is a segment to segment penalty based contact. For two segments on each side of the contact interface that are overlapping and penetrating, a consistent nodal force assembly taking into account the individual shape functions of the segments is performed, see Figure 11-16 for an illustration. A TRANSDUCER_PENALTY can be used for extract- ing forces from Mortar contacts, but the slave and master sides must then be defined through parts or part sets. In this respect the results with this contact may be more accurate, especially when considering contact with elements of higher order. By appending the suffix TIED to the CONTACT_AUTOMATIC_SURFACE_TO_SURFACE_MOR- TAR keyword or the suffix TIEBREAK_MORTAR (only OPTION = 7 and OP- TION = 9 supported) to the CONTACT_AUTOMATIC_SURFACE_TO_SUR- FACE keyword, this is treated as a tied contact interface with optional failure in the latter case. This contact is intended for implicit analysis in particular but is nevertheless supported for explicit analysis as well. For explicit analysis, the bucket sort frequency is 100 if not specified. The FORMING mortar contact, in contrast to other forming contacts, does not assume a rigid master side, but if this side consists of shell elements the normal should be oriented towards the slave side. Furthermore, no shell thickness is taken into account on the master side. The slave side is assumed to be a de- formable shell part, and the orientation of the elements does not matter. How- ever, each FORMING contact definition should be such that contact occurs with ONE deformable slave side only, which obviously leads to multiple contact definitions if two-sided contact is presumed. The AUTOMATIC contact is supported for solids, shells and beams, and here the thicknesses are taken into account both for rigid and deformable parts. Flat edge contact is supported for shell elements and contact with beams occurs on the lateral surface area as well as on the end tip. The contact assumes that the beam has a cylindrical shape with a cross sectional area coinciding with that of the underlying beam element. For the AUTOMATIC contact, the contact surface can be augmented with the aid of parameters SST and SFST for shells and beams, while SLDTHK is used for solids and thick shells. For shells/beams SST corresponds to the contact thickness of the element (MST likewise for the master side), by default this is the same as the element thickness. This parameter can be scaled with aid of SFST (SFMT for the master side) to adjust the location of the contact surface, see Figure 11-14. For solids PENMAX can be used to determine the maximum penetration and also determines the search depth for finding contact pairs, if set it should corre- spond to a characteristic thickness in the model. Also, the contact surface can be adjusted with the aid of SLDTHK if it is of importance to reduce the gap between parts, see Figure 11-14. This may be of interest if initial gaps result in free objects undergoing rigid body motion and thus preventing convergence in implicit. 4 3.5 3 2.5 2 1.5 1 0.5 0 0 IGAP=1 IGAP=2 IGAP=5 IGAP=10 0.2 0.4 0.6 0.8 1 Penetration Figure 11-15. Mortar contact stress as function of penetration For the TIED option, the criterion for tying two contact surfaces is by default that the distance should be less than 0.05 × T, i.e., by default it is within 5% of the element thickness (characteristic size for solids). In this case PENMAX can be used to set the tying distance, i.e., if PENMAX is positive then segments are tied if the distance is less than PENMAX. If initial penetrations are detected (reported in the messag file) then by default these will yield an initial contact stress corresponding to this level of penetra- tion. IGNORE > 0 can be used to prevent unwanted effects of this. IG- NORE = 2 behaves differently than from other contacts, for this option the penetrations are not tracked but the contact surface is fixed at its initial location. In addition, for IGNORE = 2, an initial contact pressure can be imposed on the interface by setting the MPAR1 parameter to the desired contact pressure. All this allows to properly eliminate any rigid body motion due to initial contact gaps. 4 Slave 1 x3 x2 O x1 Master segment Figure 11-16. Illustration of Mortar segment to segment contact A third option is IGNORE = 3, for which prestress can be applied. This allows initial penetrations to exists and they are closed during the time between zero and the value given by MPAR1, thus working pretty similar to the INTERFER- ENCE option with the exception that the closure is linear in time. A limitation with IGNORE = 3 in this context is that the initial penetrations must be small enough for the contact algorithm to detect them. Thus, for large penetrations IGNORE = 4 is recommended (this can only be used if the slave side consists of solid elements). This does pretty much the same thing as IGNORE = 3, but the user may provide a penetration depth in MPAR2. This depth must be at least as large as (and preferably in the order of) the maximum initial penetration in the contact interface or otherwise an error termination will be the result. The need for such a parameter is for the contact algorithm to have a decent chance to locate the contact surface and thus esti- mate the initial penetration. With this option the contact surfaces are pushed back and placed in incident contact at places where initial penetrations are present, this can be done for (more or less) arbitrary initial penetration depths. As for IGNORE = 3, the contact surfaces will be restored linearly in the time given by MPAR1. A problem with mortar contacts in implicit analysis could be that contact pres- sure is locally very high and leads to large enough penetrations to be released in subsequent steps. Penetration information can be requested on MINFO on *CONTROL_OUTPUT which issues a warning if there is a danger for this to happen. To prevent contact release the user may increase IGAP which penaliz- es large penetrations without affecting small penetration behavior and thereby overall implicit performance. Figure 11-15 shows the contact pressure as func- tion of penetration for the mortar contact, including the effect of increasing IGAP. It also shows that for sufficiently large penetrations the contact is not detected in subsequent steps which is something to avoid. INTERFACE TYPE ID PENCHK ELEMENT TYPE FORMULA FOR RELEASE OF PENETRATING NODAL POINT 0 1 2 1, 2, 6, 7 3, 5, 8, 9, 10 (without thickness) 3, 5, 10 (thickness), 17 and 18 a3, a5, a10, 13, 15 4 26 solid shell solid shell solid shell solid shell solid d = PENMAX if PENMAX > 0 d = 1.e+10 if PENMAX = 0 d = PENMAX if PENMAX > 0 d = 1.e+10 if PENMAX = 0 d = XPENE × thickness of solid element d = XPENE thickness of shell element d = 0.05 × minimum diagonal length d = 0.05 × minimum diagonal length d = XPENE × thickness of solid element d = XPENE × thickness of shell element d = PENMAX × thickness of solid element [default: PENMAX = 0.5] d = PENMAX × (slave thickness + master shell thickness) [default: PENMAX = 0.4] solid d = 0.5 × thickness of solid element shell solid d = 0.4 × (slave thickness + master thickness) d = PENMAX × thickness of solid element [default: PENMAX = 10.0] d = PENMAX × (slave thickness + master shell thickness) [default: PENMAX = 10.] Table 11-17. Criterion for node release for nodal points which have penetrated too far. This criterion does not apply to SOFT = 2 contact. Larger penalty stiffnesses are recommended for the contact interface which allows nodes to be released. For node-to-surface type contacts (5, 5a) the element thicknesses which contain the node determines the nodal thickness. The parameter is defined on the *CONTROL_CONTACT input. Mapping of *CONTACT keyword option to “contact type” in d3hsp: Structured Input Type ID a 13 26 i 26 a 5 a 5 a 10 13 a 3 a 3 18 17 23 16 14 15 27 25 m 5 m 10 m 3 5 5 10 20 Keyword Name AIRBAG_SINGLE_SURFACE AUTOMATIC_GENERAL AUTOMATIC_GENERAL_INTERIOR AUTOMATIC_NODES_TO_SURFACE AUTOMATIC_NODES_TO_SURFACE_TIEBREAK AUTOMATIC_ONE_WAY_SURFACE_TO_SURFACE AUTOMATIC_SINGLE_SURFACE AUTOMATIC_SURFACE_TO_SURFACE AUTOMATIC_SURFACE_TO_SURFACE_TIEBREAK CONSTRAINT_NODES_TO_SURFACE CONSTRAINT_SURFACE_TO_SURFACE DRAWBEAD ERODING_NODES_TO_SURFACE ERODING_SURFACE_TO_SURFACE ERODING_SINGLE_SURFACE FORCE_TRANSDUCER_CONSTRAINT FORCE_TRANSDUCER_PENALTY FORMING_NODES_TO_SURFACE FORMING_ONE_WAY_SURFACE_TO_SURFACE FORMING_SURFACE_TO_SURFACE NODES_TO_SURFACE NODES_TO_SURFACE_INTERFERENCE ONE_WAY_SURFACE_TO_SURFACE RIGID_NODES_TO_RIGID_BODY Structured Input Type ID 21 19 22 4 1 Keyword Name RIGID_BODY_ONE_WAY_TO_RIGID_BODY RIGID_BODY_TWO_WAY_TO_RIGID_BODY SINGLE_EDGE SINGLE_SURFACE SLIDING_ONLY p 1 SLIDING_ONLY_PENALTY 3 3 8 9 6 o 6 c 6 7 o 7 c 7 b 7 s 7 2 o 2 c 2 SURFACE_TO_SURFACE SURFACE_TO_SURFACE_INTERFERENCE TIEBREAK_NODES_TO_SURFACE TIEBREAK_SURFACE_TO_SURFACE TIED_NODES_TO_SURFACE TIED_NODES_TO_SURFACE_OFFSET TIED_NODES_TO_SURFACE_CONSTRAINED_OFFSET TIED_SHELL_EDGE_TO_SURFACE or SPOTWELD TIED_SHELL_EDGE_TO_SURFACE_OFFSET TIED_SHELL_EDGE_TO_SURFACE_CONSTRAINED_OFFSET or SPOTWELD_CONSTRAINED_OFFSET TIED_SHELL_EDGE_TO_SURFACE_BEAM_OFFSET SPOTWELD_BEAM_OFFSET or SPOTWELD_WITH_TORSION TIED_SURFACE_TO_SURFACE TIED_SURFACE_TO_SURFACE_OFFSET TIED_SURFACE_TO_SURFACE_CONSTRAINED_OFFSET *CONTACT_OPTION1_{OPTION2}_… $ $$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ $ $$$$ *CONTACT_NODES_TO_SURFACE $ $$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ $ $ Make a simple contact that prevents the nodes in part 2 from $ penetrating the segments in part 3. $ *CONTACT_NODES_TO_SURFACE $ $...>....1....>....2....>....3....>....4....>....5....>....6....>....7....>....8 $ ssid msid sstyp mstyp sboxid mboxid spr mpr 2 3 3 3 $ $ fs fd dc vc vdc penchk bt dt $ $ sfs sfm sst mst sfst sfmt fsf vsf $ $ sstype, mstype = 3 id's specified in ssid and msid are parts $ ssid = 2 use slave nodes in part 2 $ msid = 3 use master segments in part 3 $ $ Use defaults for all parameters. $ $$$$ Optional Cards A and B not specified (default values will be used). $ $ $ $$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ $ $ $$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ $ $$$$ *CONTACT_SINGLE_SURFACE $ $$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ $ $ Create a single surface contact between four parts: 28, 97, 88 and 92 $ - create a part set with set ID = 5, list the four parts $ - in the *CONTACT_SINGLE_SURFACE definition specify: $ sstyp = 2 which means the value for ssid is a part set $ ssid = 5 use part set 5 for defining the contact surfaces $ $ Additional contact specifications described below. $ *CONTACT_SINGLE_SURFACE $ $...>....1....>....2....>....3....>....4....>....5....>....6....>....7....>....8 $ ssid msid sstyp mstyp sboxid mboxid spr mpr 5 2 $ fs fd dc vc vdc penchk bt dt 0.08 0.05 10 20 40.0 $ sfs sfm sst mst sfst sfmt fsf vsf $ $ fs = 0.08 static coefficient of friction equals 0.08 $ fd = 0.05 dynamic coefficient of friction equals 0.05 $ dc = 10 exponential decay coefficient, helps specify the transition $ from a static slide to a very dynamic slide $ vdc = 20 viscous damping of 20% critical (damps out nodal $ oscillations due to the contact) $ dt = 40.0 contact will deactivate at 40 ms (assuming time unit is ms) $ $$$$ Optional Cards A and B not specified (default values will be used). $ $ *SET_PART_LIST $ sid 5 $ pid1 pid2 pid3 pid4 28 97 88 92 $ $$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ $ $$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ $ $$$$ *CONTACT_DRAWBEAD $ $$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ $ $ Define a draw bead contact: $ - the draw bead is to be made from the nodes specified in node set 2 $ - the master segments are to be those found in the box defined by box 2 $ that are in part 18 $ - include slave and master forces in interface file (spr, mpr = 1) $ *CONTACT_DRAWBEAD $ $...>....1....>....2....>....3....>....4....>....5....>....6....>....7....>....8 $ ssid msid sstyp mstyp sboxid mboxid spr mpr 2 18 4 3 2 1 1 $ $ fs fd dc vc vdc penchk bt dt 0.10 $ $ sfs sfm sst mst sfst sfmt fsf vsf $ $$$$ Card 4 required because it's a drawbead contact $ $ lcdidrf lcidnf dbdth dfscl numint 3 0.17436 2.0 $ $ lcdidrf = 3 load curve 3 specifies the bending component of the $ restraining force per unit draw bead length $ dbdth = 0.17436 draw bead depth $ dfscl = 2.0 scale load curve 3 (lcdidrf) by 2 $ $$$$ Optional Cards A and B not specified (default values will be used). $ *DEFINE_BOX $ boxid xmm xmx ymn ymx zmn zmx 2 0.000E+00 6.000E+00 6.000E+00 1.000E+02-1.000E+03 1.000E+03 $ *SET_NODE_LIST $ sid da1 da2 da3 da4 2 $ nid1 nid2 nid3 nid4 nid5 nid6 nid7 nid8 2580 2581 2582 2583 2584 2585 2586 2587 2588 2589 2590 $ *DEFINE_CURVE $ lcid sidr scla sclo offa offo 3 $ a o $ DEPTH FORC/LGTH 0.000E+00 0.000E+00 1.200E-01 1.300E+02 1.500E-01 2.000E+02 1.800E-01 5.000E+02 *CONTACT This card associates a wear model to a contact interface for post-processing wear quantities. This card does not affect the results of a simulation. Wear is associated to friction so the frictional coefficient must be nonzero for the associated contact interface. This feature calculates the wear depth, sliding distance and possibly user defined wear history variables according to the specified model and writes it to the intfor database for post- processing. Note that this data is not written unless the parameter NWEAR and/or NWUSR are set on the *DATABASE_EXTENT_INTFOR card. 𝐻-adaptive remeshing is supported with this feature. Implicit analysis is supported, for which mortar is the preferred contact. Card 1 1 2 Variable CID WTYPE Type I I 3 P1 F 4 P2 F 5 P3 F 6 P4 F 7 P5 F 8 P6 F Default none none none none none none none none User Defined Wear Parameter Cards. Define as many cards as needed to define P1 parameters if and only if WTYPE.LT.0. Card n 1 Variable W1 2 W2 3 W3 4 W4 5 W5 6 W6 7 W7 8 W8 Type F F F F F F F F Default none none none none none none none none VARIABLE DESCRIPTION CID Contact interface ID, see *CONTACT_… VARIABLE DESCRIPTION WTYPE Wear law LT.0: User defined wear law, value specifies type used in subroutine. EQ.0: Archard’s wear law. P1 First wear parameter WTYPE.EQ.0: Dimensionless scale factor 𝑘. If negative the ID with absolute value specifies a 𝑘 = 𝑘(𝑝, 𝑑 ̇) as a function of contact pressure 𝑝 ≥ 0 and relative sliding velocity 𝑑 ̇≥ 0. table WTYPE.LT.0: Number of user wear parameters for this interface. P2 Second wear parameter WTYPE.EQ.0: Slave surface hardness parameter 𝐻𝑠. If negative the absolute value specifies a curve ID with 𝐻𝑠 = 𝐻𝑠(𝑇𝑠) as function of slave node tempera- ture 𝑇𝑠. WTYPE.LT.0: Number of user wear history variables per contact node, these can be output to the intfor file, see NWUSR on *DATABASE_EXTENT_- INTFOR. P3 Third wear parameter WTYPE.EQ.0: Master surface hardness parameter 𝐻𝑚. If negative the absolute value specifies a curve ID with 𝐻𝑚 = 𝐻𝑚(𝑇𝑚) as function of master node temperature 𝑇𝑚. WTYPE.LT.0: Not used. P4 - P6 Not used. WN Nth user defined wear parameter. Remarks: Archard’s wear law (WTYPE.EQ.0) states that the wear depth 𝑤 at a contact point evolves with time as 𝑤̇ = 𝑘 𝑝𝑑 ̇ where 𝑘 > 0 is a dimensionless scale factor, 𝑝 ≥ 0 is the contact interface pressure, 𝑑 ̇≥ 0 is the relative sliding velocity of the points in contact and 𝐻 > 0 is the surface hardness (force per area). The wear depth for a node in contact is incremented in accordance with this formula, accounting for different hardness of the slave and master side, 𝐻𝑠 and 𝐻𝑚, respectively. By using negative numbers for wear parameters P1, P2 or P3, the corresponding parameter is defined by a table or a curve. For P1, the value of 𝑘 is taken from a table with contact pressure 𝑝 and sliding velocity 𝑑 ̇ as arguments, while for P2 or P3, the corresponding hardness 𝐻 is taken from curves with the associated contact nodal temperature 𝑇 as argument. That is, the slave side hardness will be a function of the slave side temperature, and vice versa. Customized wear laws may be specified as a user-defined subroutine called userwear. This subroutine is called when WTYPE < 0. This subroutine is passed wear parameters for this interface as well as number of wear history variables per contact node. The wear parameters are defined on additional cards and the history variables are updated in the user subroutine. The history variables can be output to the intfor file, see NWUSR on *DATABASE_EXTENT_INTFOR. WTYPE may be used to distinguish between different wear laws, and consequently any number of different laws can be implemented within the same subroutine. For more information, we refer to the source code which contains extensive commentaries and two sample wear laws. Only one wear law per contact interface can be specified. The procedure for activating this feature involves 1. Using the present keyword to associate wear to a contact interface 2. Setting NWEAR and/or NWUSR on the *DATABASE_EXTENT_INTFOR card. 3. Having a contact interface with friction of a type that is supported.. If SOFT = 2 on optional card A of the contact data, then any valid keyword option is sup- ported. If SOFT = 0 or SOFT = 1, then the following list is supported. *CONTACT_FORMING_ONE_WAY_SURFACE_TO_SURFACE *CONTACT_FORMING_SURFACE_TO_SURFACE *CONTACT_AUTOMATIC_SURFACE_TO_SURFACE *CONTACT_FORMING_SURFACE_TO_SURFACE_MORTAR *CONTACT_AUTOMATIC_SURFACE_TO_SURFACE_MORTAR *CONTACT_AUTOMATIC_SINGLE_SURFACE_MORTAR 1. _SMOOTH option is not supported 2. MPP “groupable” option is not supported *CONTACT_ADD_WEAR See also *DATABASE_EXTENT_INTFOR for general guidelines related to the intfor database. *CONTACT Purpose: This feature allows for automatic move of a master surface in a contact definition to close an unspecified gap between a slave and the master surface. The gap may be caused as a result of an initial gravity loading on the slave part. The gap will be closed on a specified time to save CPU time. The master surface in metal forming application will typically be the upper cavity and the slave part will be the blank. This feature is applicable only for sheet metal forming application. Cards 1 Variable 1 ID 2 3 4 5 6 7 8 CONTID VID LCID ATIME OFFSET Type I I I Default none none none I 0 F F 0.0 0.0 VARIABLE DESCRIPTION ID Move ID for this automatic move input. CONTID VID LCID GT.0: velocity controlled tool kinematics (the variable VAD = 0 in *BOUNDARY_PRESCRIBED_MOTION_RIGID) LT.0: displacement controlled tool kinematics (VAD = 2) Contact ID, as in *CONTACT_FORMING_...._ID, which defines the slave and master part set IDs. Vector ID of a vector oriented in the direction of movement of the master surface, as in *DEFINE_VECTOR. The origin of the vector is unimportant since the direction cosines of the vector are computed and used. Load curve defining tooling kinematics, either by velocity versus time or by displacement versus time. This load curve will be adjusted automatically during a simulation to close the empty tool travel. ATIME Activation time defining the moment the master surface (tool) to be moved. OFFSET *CONTACT_AUTO_MOVE DESCRIPTION Time at which a master surface will move to close a gap distance, which may happen following the move of another master surface. This is useful in sequential multiple flanging or press hemming simulation. Simulation time (CPU) is much faster based on the shortened tool travel (no change to the termination time). Example: gravity loading and closing with implicit static Referring to the partial input deck below and Figure 11-18, a combined simulation of gravity loading and binder closing of a fender outer is demonstrated on the NUMISHEET 2002 benchmark. In this multi-step implicit static set up, the blank is allocated 0.3 “time” units (3 implicit steps for DT0 = 0.1) to be loaded with gravity. At the end of gravity loading, a gap of 12mm was created between the upper die and the blank, Figure 11-19. The upper die is set to be moved at 0.3 “time” units, closing the gap caused by the gravity effect on the blank (Figure 11-20 left). An intermediate closing state is shown at t = 0.743 (Figure 11-20 right) while the final completed closing is shown in Figure 11-21. It is noted that the upper die is controlled with displacement (VAD = 2) in a shape of a right triangular in the displacement versus “time” space as defined by load curve #201, and the ID in *CONTACT_AUTO_MOVE is set to “-1”. *PARAMETER R grvtime 0.3 R endtime 1.0 R diemv 145.45 *CONTROL_TERMINATION &endtime *CONTROL_IMPLICIT_FORMING 2,2,100 *CONTROL_IMPLICIT_GENERAL $ IMFLAG DT0 1 0.10 *CONTROL_ACCURACY 1 2 *CONTACT_FORMING_ONE_WAY_SURFACE_TO_SURFACE_ID 11 .... .... .... $---+----1----+----2----+----3----+----4----+----5----+----6----+----7----+----8 *BOUNDARY_PRESCRIBED_MOTION_RIGID $# pid dof vad lcid sf vid death birth 2 3 2 201 -1.000000 0 0.0 0.000 *CONTACT_AUTO_MOVE $ ID ContID VID LCID ATIME -1 11 89 201 &grvtime *DEFINE_VECTOR 89,0.0,0.0,0.0,0.0,0.0,-10.0 *DEFINE_CURVE 201 0.0,0.0 &grvtime,0.0 1.0,&diemv Similarly, “velocity” controlled tool kinematics is also enabled. In the example keyword below, the “velocity” profile is ramped up initially and then kept constant. It is noted that the variable VAD in *BOUNDARY is set to “0”, and ID in *CONTACT_- AUTO_MOVE is set to positive “1” indicating it is a velocity boundary condition. *PARAMETER R grvtime 0.3 R tramp 0.001 R diemv 145.45 R clsv 1000.0 *PARAMETER_EXPRESSION R tramp1 tramp+gravtime R endtime tramp1+(abs(diemv)-0.5*clsv*tramp)/clsv *CONTACT_FORMING_ONE_WAY_SURFACE_TO_SURFACE_ID 11 .... .... $---+----1----+----2----+----3----+----4----+----5----+----6----+----7----+----8 *BOUNDARY_PRESCRIBED_MOTION_RIGID $# pid dof vad lcid sf vid death birth 2 3 0 201 -1.000000 0 0.0 0.000 *CONTACT_AUTO_MOVE $ ID ContID VID LCID ATIME 1 11 89 201 &grvtime *DEFINE_VECTOR 89,0.0,0.0,0.0,0.0,0.0,-10.0 *DEFINE_CURVE 201 0.0,0.0 0.2,0.0 &tramp1,&clsv &endtime,&clsv Example: tool delay in sequential flanging process with explicit dynamic: The following example demonstrates the use of the variable OFFSET. As shown in Figure 11-22 (left), a total of 5 flange steels are auto-positioned initially according to the initial blank shape. Upon closing of the pressure pad, a first set of 4 flanging steels move to home completing the first stage of the stamping process (Figure 11-22 right). The gap created by the completion of the first flanging process is closed automatically at a time defined using variables ATIME/OFFSET (Figure 11-23 left). During the second stage of the process, flanging steel &flg5pid moves to home completing the final flanging (Figure 11-23 right). An excerpt from the input deck for this model can be found below. This deck was created using LS-PrePost’s eZ-Setup feature (http://ftp.lstc.com/- anonymous/outgoing/lsprepost/4.0/metalforming/), with two additional keywords added:*CONTACT_AUTO_MOVE and *DEFINE_VECTOR. Flanging steel #5 is set to move in a cam angle defined by vector #7 following the completion of the flanging (straight down) process of flanging steel #2. The variables ATIME and OFFSET in *CONTACT_AUTO_MOVE are both defined as &endtime4, which is calculated based on the automatic positioning of tools/blank using *CON- TROL_FORMING_AUTOPOSITION. At defined time, flanging steel #5 ‘jumps’ into position to where it just comes into contact with the partially formed down-standing flange, saving some CPU times (Figure 11-23 left). Flanging steel #5 continues to move to its home position completing the simulation (Figure 11-23 right). The CPU time savings is 27% in this case. *KEYWORD *PARAMETER ... *PART &flg5pid &flg5sec &flg5mid ... $---+----1----+----2----+----3----+----4----+----5----+----6----+----7----+----8 $ Local coordinate system for flanging steel #5 move direction *DEFINE_COORDINATE_SYSTEM $# cid xo yo zo xl yl zl &flg5cid -5.09548 27.6584 -8.98238 -5.43587 26.8608 -9.48034 $# xp yp zp -5.82509 27.5484 -8.30742 $---+----1----+----2----+----3----+----4----+----5----+----6----+----7----+----8 $ Auto positioning *CONTROL_FORMING_AUTOPOSITION_PARAMETER_SET $ SID CID DIR MPID POSITION PREMOVE THICK PARORDER ... &flg5sid &flg5cid 3 &blk1sid -1 &bthick flg5mv *PART_MOVE $ PID XMOV YMOV ZMOV CID IFSET &flg5sid 0.0 0.0 &flg5mv&flg5cid 1 ... *MAT_RIGID $ MID RO E PR N COUPLE M ALIAS &flg5mid 7.830E-09 2.070E+05 0.28 $ CMO CON1 CON2 -1 &flg5cid 110111 $LCO or A1 A2 A3 V1 V2 V3 &flg5cid $---+----1----+----2----+----3----+----4----+----5----+----6----+----7----+----8 *CONTACT_AUTO_MOVE $ ID CONTID VID LCID ATIME OFFSET 1 7 7 10 &endtim4 &endtim4 *DEFINE_VECTOR $ VID XT YT ZT XH YH ZH 7 0.0 0.0 0.0-0.5931240 0.5930674-0.5444952 *CONTACT_FORMING_ONE_WAY_SURFACE_TO_SURFACE_ID $ CID 7 $ SSID MSID SSTYP MSTYP SBOXID MBOXID SPR MPR &blk1sid &flg5sid 2 2 1 1 $ FS FD DC VC VDC PENCHK BT DT ... $---+----1----+----2----+----3----+----4----+----5----+----6----+----7----+----8 $ Tool kinematics $ -------------------------closing *BOUNDARY_PRESCRIBED_MOTION_RIGID_local ... &flg5pid 3 0 4 1.0 0 &endtim4 $ -------------------------flanging *BOUNDARY_PRESCRIBED_MOTION_RIGID_local ... &flg5pid 3 0 10 1.0 0 &endtim4 $---+----1----+----2----+----3----+----4----+----5----+----6----+----7----+----8 *END *CONTACT This feature is implemented in LS-DYNA Revision 64066 and later releases. The variable OFFSET is in Revision 77137 and later releases. Sheet blank Upper die cavity Lower binder Lower punch Figure 11-18. Initial parts auto-positioned at t = 0.0. 12mm gap Gravity loaded sheet blank Figure 11-19. Gravity loading on blank at t = 0.2. Figure 11-20. Upper die move down at t = 0.3 closing the gap (left); continue closing at t = 0.743 (right). Figure 11-21. Closing complete at t = 1.0. Flanging Steel #2: 0 Flanging steel #5: &flg5pid Time = 0 Time = 0.00954 ATIME, OFFSET, &endtime4 Figure 11-22. A sequential flanging process (left); first set of flanging steels reaching home (right). Time = 0.018743 Time = 0.026022 Gap closes. This happens in an “instant,” meaning the time step does not increment. &flg5pid finish flanging Figure 11-23. Closing the empty travel (left); flanging steel &flg5pid completes flanging process (right). *CONTACT_COUPLING Purpose: Define a coupling surface for MADYMO to couple LS-DYNA with deformable and rigid parts within MADYMO. In this interface, MADYMO computes the contact forces acting on the coupling surface, and LS-DYNA uses these forces in the update of the motion of the coupling surface for the next time step. Contact coupling can be used with other coupling options in LS-DYNA. 2 3 4 5 6 7 8 Card 1 Variable 1 ID Type I Default required Set Cards. Include on card for each coupled set. The next "*" card terminates this input. Card 2 1 2 3 4 5 6 7 8 Variable SID STYPE Type I I Default required 0 VARIABLE DESCRIPTION SID Set ID for coupling. See Remark 1 below. STYPE Set type: EQ.0: part set EQ.1: shell element set EQ.2: solid element set EQ.3: thick shell element set *CONTACT 1. Only one coupling surface can be defined. If additional surfaces are defined, the coupling information will be added to the first definition. 2. The units and orientation can be converted by using the CONTROL_COU- PLING keyword. It is not necessary to use the same system of units in MADY- MO and in LS-DYNA if unit conversion factors are defined. *CONTACT_ENTITY Purpose: Define a contact entity. Geometric contact entities treat the impact between a deformable body defined as a set of slave nodes or nodes in a shell part set and a rigid body. The shape of the rigid body is determined by attaching geometric entities. Contact is treated between these geometric entities and the slave nodes using a penalty formulation. The penalty stiffness is optionally maximized within the constraint of the Courant criterion. As an alternative, a finite element mesh made with shells can be used as geometric entity. Also, axisymmetric entities with arbitrary shape made with multi-linear polygons are possible. The latter is particularly useful for metalforming simulations. WARNING: If the problem being simulated involves dynamic motion of the entity, care should be taken to insure that the inertial properties of the entity are correct. It may be necessary to use the *PART_INERTIA option to specify these properties. The data set for *CONTACT_ENTITY consists of 5 cards: Card 1 1 2 3 4 Variable PID GEOTYP SSID SSTYP Type I I I Default required required required I 0 5 SF F 1. 6 DF F 0. 7 CF F 0. 8 INTORD I 0 VARIABLE PID DESCRIPTION Part ID of the rigid body to which the geometric entity is attached, see *PART. GEOTYPE = 1: Infinite Plane GEOYPE = 2: Sphere Z' X' Y' GEOYPE = 3: Infinite Cylinder GEOTYPE = 4: Hyperellipsoid Figure 11-24. Contact Entities. VARIABLE DESCRIPTION GEOTYP Type of geometric entity: EQ.1: plane, EQ.2: sphere, EQ.3: cylinder, EQ.4: ellipsoid, EQ.5: torus, EQ.6: CAL3D/MADYMO Plane, see Appendix I, EQ.7: CAL3D/MADYMO Ellipsoid, see Appendix I, EQ.8: VDA surface, see Appendix L, EQ.9: rigid body finite element mesh (shells only), EQ.10: finite plane, EQ.11: load curve defining line as surface profile of axisym- metric rigid bodies. Y' Z' Z' Y' X' g2 GEOTYPE = 5: Torus GEOTYPE = 10: Finite Plane X' g1 Z' - axis of symmetry Load Curve X' GEOTYPE = 11: Load Curve Y' Figure 11-25. More contact entities. VARIABLE DESCRIPTION SSID Slave set ID, see *SET_NODE_OPTION, *PART, or *SET_PART. SSTYP Slave set type: EQ.0: node set, EQ.1: part ID, EQ.2: part set ID. SF DF Penalty scale factor. Useful to scale maximized penalty. Damping option, see description for *CONTACT_OPTION: EQ.0: no damping, GT.0: viscous damping in percent of critical, e.g., 20 for 20% damping, LT.0: DF must be a negative integer. -DF is the load curve ID giving the damping force versus relative normal velocity . VARIABLE DESCRIPTION CF Coulomb friction coefficient. See remark 2 below. EQ.0: no friction GT.0: constant friction coefficient LT.0: CF must be a negative integer. -CF is the load curve ID giving the friction coefficient versus time. INTORD Integration order (slaved materials only). This option is not available with entity types 8 and 9 where only nodes are checked: EQ.0: check nodes only, EQ.1: 1 point integration over segments, EQ.2: 2 × 2 integration, EQ.3: 3 × 3 integration, EQ.4: 4 × 4 integration, EQ.5: 5 × 5 integration. This option allows a check of the penetration of the rigid body into the deformable (slaved) material. Then virtual nodes at the location of the integration points are checked. Remarks: 1. The optional load curves that are defined for damping versus relative normal velocity and for force versus normal penetration should be defined in the posi- tive quadrant. The sign for the damping force depends on the direction of the relative velocity and the treatment is symmetric if the damping curve is in the positive quadrant. If the damping force is defined in the negative and positive quadrants, the sign of the relative velocity is used in the table look-up. 2. If at any time the friction coefficient is >= 1.0, the force calculation is modified to a constraint like formulation which allows no sliding. This is only recom- mended for entities with constrained motion since the mass of the entity is assumed to be infinite. Variable 1 BT Type F 2 DT F Default 0. 1.E+20 3 SO I 0 4 GO I 0 *CONTACT_ENTITY 5 6 7 8 ITHK SPR I 0 I 0 VARIABLE DESCRIPTION BT DT SO GO Birth time Death time Flag to use penalty stiffness as in surface-to-surface contact: EQ.0: contact entity stiffness formulation, EQ.1: surface to surface contact method, EQ.2: normal force is computed via a constraint-like method. The contact entity is considered to be infinitely massive, so this is recommended only for entities with constrained motion. LT.0: SO must be an integer: -SO is the load curve ID giving the force versus the normal penetration. Flag for automatic meshing of the contact entity for entity types 1- 5 and 10-11. GO = 1 creates null shells for visualization of the contact entity. Note these shells have mass and will affect the mass properties of the rigid body PID unless *PART_INERTIA is used for the rigid body. EQ.0: mesh is not generated, EQ.1: mesh is generated. ITHK Flag for considering thickness for shell slave nodes (applies only to entity types 1, 2, 3; SSTYP must be set to zero). EQ.0: shell thickness is not considered, EQ.1: shell thickness is considered, VARIABLE SPR Card 3 Variable 1 XC Type F Default 0. Card 4 Variable 1 BX Type F Default 0. DESCRIPTION Include interface force files, valid only when SSTYP > 0: the slave side in *DATABASE_BINARY_INTFOR EQ.1: slave side forces included. 4 AX F 0. 5 AY F 0. 4 5 6 AZ F 0 6 7 8 7 8 2 YC F 0. 2 BY F 0. 3 ZC F 0. 3 BZ F 0. VARIABLE DESCRIPTION XC YC ZC AX AY AZ BX BY 𝑥-center, 𝑥𝑐, see remarks below. 𝑦-center, 𝑦𝑐, see remarks below. 𝑧-center, 𝑧𝑐. See remarks below. 𝑥-direction for local axis 𝐀, 𝐴𝑥, see remarks below. y-direction for local axis 𝐀, 𝐴𝑦, see remarks below. z-direction for local axis 𝐀, 𝐴𝑧, see remarks below. 𝑥-direction for local axis 𝐁, Bx, see remarks below. 𝑦-direction for local axis 𝐁, 𝐵𝑦, see remarks below. VARIABLE DESCRIPTION BZ 𝑧-direction for local axis 𝐁, 𝐵𝑧, see remarks below. Remarks:: 1. The coordinates, (𝑥𝑐, 𝑦𝑐, 𝑧𝑐) are the positions of the local origin of the geometric entity in global coordinates. The entity’s local A-axis is determined by the vector (𝐴𝑥, 𝐴𝑦, 𝐴𝑧) and the local 𝐵-axis by the vector (𝐵𝑥, 𝐵𝑦, 𝐵𝑧). 2. Cards 3 and 4 define a local to global transformation. The geometric contact entities are defined in a local system and transformed into the global system. For the ellipsoid, this is necessary because it has a restricted definition for the local position. For the plane, sphere, and cylinder, the entities can be defined in the global system and the transformation becomes (𝑥𝑐, 𝑦𝑐, 𝑧𝑐) = (0,0,0), (𝐴𝑥, 𝐴𝑦, 𝐴𝑧) = (1,0,0), and (𝐵𝑥, 𝐵𝑦, 𝐵𝑧) = (0,1,0). Card 5 1 Variable INOUT Type Default I 0 2 G1 F 0. 3 G2 F 0. 4 G3 F 0. 5 G4 F 0. 6 G5 F 0. 7 G6 F 0. 8 G7 F 0. VARIABLE INOUT G1 G2 G3 G4 G5 DESCRIPTION In-out flag. Allows contact from the inside or the outside (default) of the entity: EQ.0: slave nodes exist outside of the entity, EQ.1: slave nodes exist inside the entity. Entity coefficient 𝑔1 (CAL3D/MADYMO plane or ellipse number) for coupled analysis . Entity coefficient 𝑔2, see remarks below. Entity coefficient 𝑔3, see remarks below. Entity coefficient 𝑔4, see remarks below. Entity coefficient 𝑔5, see remarks below. VARIABLE DESCRIPTION G6 G7 Entity coefficient 𝑔6, see remarks below. Entity coefficient 𝑔7, see remarks below. Remarks: Figures 11-24 and 11-25 show the definitions of the geometric contact entities. The relationships between the entity coefficients and the Figure 11-25 and 11-24 variables are as described below. Note that (𝑃𝑥, 𝑃𝑦, 𝑃𝑧) defines a point and (𝑄𝑥, 𝑄𝑦, 𝑄𝑧) is a direction vector. GEOTYP = 1 𝑔1 = 𝑃𝑥 𝑔2 = 𝑃𝑦 𝑔3 = 𝑃𝑧 𝑔4 = 𝑄𝑥 𝑔5 = 𝑄𝑦 𝑔6 = 𝑄𝑧 𝑔7 = 𝐿 If automatic generation is used, a square plane of length L on each edge is generated which represents the infinite plane. If generation is inactive, then g7 may be ignored. GEOTYP = 2 GEOTYP = 3 𝑔1 = 𝑃𝑥 𝑔2 = 𝑃𝑦 𝑔3 = 𝑃𝑧 𝑔1 = 𝑃𝑥 𝑔2 = 𝑃𝑦 𝑔3 = 𝑃𝑧 𝑔4 = 𝑟 𝑔4 = 𝑄𝑋 𝑔5 = 𝑄𝑦 𝑔6 = 𝑄𝑧 𝑔7 = 𝑟 If automatic generation is used, a cylinder of length √𝑄x generated which represents the infinite cylinder. 2 + 𝑄𝑦 2 + 𝑄z 2 and radius r is GEOTYP = 4 𝑔1 = 𝑃𝑥 𝑔2 = 𝑃𝑦 𝑔3 = 𝑃𝑧 𝑔4 = 𝑎 𝑔5 = 𝑏 𝑔6 = 𝑐 𝑔7 = 𝑛 (order of the ellipsoid) *CONTACT_ENTITY 𝑔1 = Radius of torus 𝑔2 = 𝑟 𝑔3 = number of elements along minor circumference 𝑔4 = number of elements along major circumference 𝑔1 = Blank thickness (option to override true thickness) 𝑔2 = Scale factor for true thickness (optional) 𝑔3 = Load curve ID defining thickness versus time. (optional) GEOTYP = 8 GEOTYP = 9 𝑔1 = Shell thickness (option to override true thickness). NOTE: The shell thickness specification is necessary if the slave surface is generated from solid elements. 𝑔2 = Scale factor for true thickness (optional) 𝑔3 = Load curve ID defining thickness versus time. (optional) GEOTYP = 10 𝑔1 = Length of edge along X′ axis 𝑔2 = Length of edge along Y′ axis GEOTYP = 11 𝑔1 = Load curve ID defining axisymmetric surface profile about Z-axis. Load curves defined by the keywords *DEFINE_CURVE or *DE- FINE_CURVE_ENTITY can be used. 𝑔2 = Number of elements along circumference EQ.0: default set to 10 𝑔3 = Number of elements along axis EQ.0: default set to 20 EQ.-1: the elements generated from points on the load curve 𝑔4 = Number of sub divisions on load curve used to calculate contact EQ.0: default set to 1000 *CONTACT Purpose: Define contact interaction between the segment of a GEBOD dummy and parts or nodes of the finite element model. This implementation follows that of the contact entity, however, it is specialized for the dummies. Forces may be output using the *DATABASE_GCEOUT command. See *COMPONENT_GEBOD and Appendix N for further details. Conventional *CONTACT_OPTION treatment (surface-to-surface, nodes-to-surface, etc.) can also be applied to the segments of a dummy. To use this approach it is first necessary to determine part ID assignments by running the model through LS-DYNA's initialization phase. The following options are available and refer to the ellipsoids which comprise the dummy. Options involving HAND are not applicable for the child dummy since its lower arm and hand share a common ellipsoid. LOWER_TORSO MIDDLE_TORSO UPPER_TORSO NECK HEAD RIGHT_LOWER_ARM LEFT_HAND RIGHT_HAND LEFT_UPPER_LEG RIGHT_UPPER_LEG LEFT_SHOULDER LEFT_LOWER_LEG RIGHT_SHOULDER RIGHT_LOWER_LEG LEFT_UPPER_ARM RIGHT_UPPER_ARM LEFT_LOWER_ARM LEFT_FOOT RIGHT_FOOT 1 2 3 Variable DID SSID SSTYP Type I I I 4 SF F 5 DF F 6 CF F Default required required required 1. 20. 0.5 *CONTACT_GEBOD 7 8 INTORD I 0 VARIABLE DESCRIPTION DID SSID Dummy ID, see *COMPONENT_GEBOD_OPTION. Slave set ID, see *SET_NODE_OPTION, *PART, or *SET_PART. SSTYP Slave set type: EQ.0: node set, EQ.1: part ID, EQ.2: part set ID. SF DF Penalty scale factor. Useful to scale maximized penalty. Damping option, see description for *CONTACT_OPTION: EQ.0: no damping, GT.0: viscous damping in percent of critical, e.g., 20 for 20% damping, LT.0: DF must be an integer. -DF is the load curve ID giving the damping force versus relative normal velocity . CF Coulomb friction coefficient . Assumed to be constant. VARIABLE DESCRIPTION INTORD Integration order (slaved materials only). EQ.0: check nodes only, EQ.1: 1 point integration over segments, EQ.2: 2 × 2 integration, EQ.3: 3 × 3 integration, EQ.4: 4 × 4 integration, EQ.5: 5 × 5 integration. This option allows a check of the penetration of the dummy segment into the deformable (slaved) material. Then virtual nodes at the location of the integration points are checked. 4 5 6 7 8 Card 2 Variable 1 BT Type F 2 DT F Default 0. 1.E+20 3 SO I 0 VARIABLE DESCRIPTION Birth time Death time Flag to use penalty stiffness as in surface-to-surface contact: EQ.0: contact entity stiffness formulation, EQ.1: surface to surface contact method, LT.0: In this case SO must be an integer. |SO| gives the load curve ID giving the force versus the normal penetration. BT DT SO Remarks: 1. The optional load curves that are defined for damping versus relative normal velocity and for force versus normal penetration should be defined in the posi- tive quadrant. The sign for the damping force depends on the direction of the relative velocity and the treatment is symmetric if the damping curve is in the positive quadrant. If the damping force is defined in the negative and positive quadrants, the sign of the relative velocity is used in the table look-up. 2. Insofar as these ellipsoidal contact surfaces are continuous and smooth it may be necessary to specify Coulomb friction values larger than those typically used with faceted contact surfaces. *CONTACT_GUIDED_CABLE_{OPTION1}_{OPTION2} Purpose: Define a sliding contact that guides 1D elements, such as springs, trusses, and beams, along a path defined by a set of nodes. Only one 1D element can be in contact with any given node in the node set at a given time. If for some reason, a node is in contact with multiple 1D elements, one guided contact definition must be used for each contact. The ordering of the nodal points and 1D elements in the input is arbitrary. OPTION1 specifies that a part set ID is given with the single option: <BLANK> SET If not used a part ID is assumed. OPTION2 specifies that the first card to read defines the heading and ID number of the contact interface and takes the single option: ID Title Card. Additional card for ID keyword option. Title 1 2 3 4 5 6 7 8 Variable CID Type I HEADING A70 VARIABLE DESCRIPTION CID Contact interface ID. This must be a unique number. HEADING Interface descriptor. It is suggested that unique descriptions be used. Card 1 1 2 3 4 5 6 7 8 Variable NSID PID/PSID SOFT SSFAC FRIC Type I I Default none none I 0 F F 1.0 none VARIABLE DESCRIPTION NSID Node set ID that guides the 1D elements. PID/PSID Part ID or part set ID if SET is included in the keyword line. SOFT Flag for soft constraint option. Set to 1 for soft constraint. SSFAC Stiffness scale factor for penalty stiffness value. The default value is unity. This applies to SOFT set to 0 and 1. FRIC Contact friction. *CONTACT Purpose: Define interior contact for solid elements. Frequently, when soft materials are compressed under high pressure, the solid elements used to discretize these materials may invert leading to negative volumes and error terminations. In order to keep these elements from inverting, it is possible to consider interior contacts between layers of interior surfaces made up of the faces of the solid elements. Since these interior surfaces are generated automatically, the part (material) ID’s for the materials of interest are defined here, prior to the interface definitions. Define as many cards as necessary. Input ends at the next * card. Multiple instances of this keyword may appear in the input. 1 2 3 4 5 6 7 8 Variable PSID1 PSID2 PSID3 PSID4 PSID5 PSID6 PSID7 PSID8 Type I I I I I I I I Default none none none none none none none none VARIABLE DESCRIPTION PSID* Part set ID for which interior contact is desired. Four attributes should be defined for each part set: Attribute 1: PSF, penalty scale factor (Default = 1.00). Attribute 2: Activation factor, Fa (Default = 0.10). When the crushing of the element reaches Fa times the initial thickness the contact algorithm begins to act. Attribute 3: ED, Optional modulus for interior contact stiffness. Attribute 4: TYPE, Formulation for interior contact. EQ.1.0: Default, recommended for uniform compression EQ.2.0: Designed to control the combined modes of shear and compression. Works for type 1 brick formulation and type 10 tetrahedron formulation. Define each part set with the *SET_PART_COLUMN option to specify independent attribute values for each part in the part set, Remarks: The interior penalty is determined by the formula: 𝐾 = SLSFAC × PSF × Volume 3⁄ × E Min. Thickness where SLSFAC is the value specified on the *CONTROL_CONTACT card , volume is the volume of the brick element, E is a constitutive modulus, and min. thickness is approximately the thickness of the solid element through its thinnest dimension. If ED, is defined above the interior penalty is then given instead by: 𝐾 = 3⁄ × ED Volume Min. Thickness where the scaling factors are ignored. Generally, ED should be taken as the locking modulus specified for the foam constitutive model. Caution should be observed when using this option since if the time step size is too large an instability may result. The time step size is not affected by the use of interior contact. *CONTACT Purpose: Define rigid surface contact. The purpose of rigid surface contact is to model large rigid surfaces, e.g., road surfaces, with nodal points and segments that require little storage and are written out at the beginning of the binary databases. The rigid surface motion, which can be optionally prescribed, is defined by a displacement vector which is written with each output state. The nodal points defining the rigid surface must be defined in the *NODE_RIGID_SURFACE section of this manual. These rigid nodal points do not contribute degrees-of-freedom. Card 1 1 2 3 4 Variable CID PSID BOXID SSID Type I I Default none none Card 2 1 2 I 0 3 5 FS F I none 0. 6 FD F 0. 7 DC F 0. 8 VC F 0. 4 5 6 7 8 Variable LCIDX LCIDY LCIDZ FSLCID FDLCID Type Default I 0 Card 3 1 I 0 2 I 0 3 I 0 4 I 0 5 6 7 8 Variable SFS STTHK SFTHK XPENE BSORT CTYPE Type F F F F I Default 1.0 0.0 1.0 4.0 10 I 0 VARIABLE DESCRIPTION CID Contact interface ID. This must be a unique number. VARIABLE DESCRIPTION PSID BOXID SSID FS FD DC VC LCIDX LCIDY Part set ID of all parts that may contact the rigid surface. See *SET_PART. Include only nodes of the part set that are within the specified box, see *DEFINE_BOX, in contact. If BOXID is zero, all nodes from the part set, PSID, will be included in the contact. Segment set ID defining the rigid surface. See *SET_SEGMENT. Static coefficient of friction. The frictional coefficient is assumed to be dependent on the relative velocity 𝑣rel of the surfaces in contact, 𝜇𝑐 = FD + (FS − FD)𝑒−DC∣𝑣rel∣. If FSLCID is defined, see below, then FS is overwritten by the value from the load curve. Dynamic coefficient of friction. The frictional coefficient is assumed to be dependent on the relative velocity 𝑣rel of the surfaces in contact, 𝜇𝑐 = FD + (FS − FD)𝑒−DC∣𝑣rel∣. If FDLCID is defined, see below, then FD is overwritten by the value from the load curve. Exponential decay coefficient. The frictional coefficient is assumed to be dependent on the relative velocity 𝑣rel of the surfaces in contact 𝜇𝑐 = FD + (FS − FD)𝑒−DC∣𝑣rel∣. Coefficient for viscous friction. This is necessary to limit the friction force to a maximum. A limiting force is computed, 𝐹lim = VC × 𝐴cont. 𝐴cont being the area of the segment contacted by the node in contact. The suggested value for VC is to use the yield stress in where σo is the yield stress of the contacted shear VC = 𝜎𝑜 √3 material. Load curve ID defining x-direction motion. If zero, there is no motion in the x-coordinate system. Load curve ID defining y-direction motion. If zero, there is no motion in the y-coordinate system. VARIABLE DESCRIPTION Load curve ID defining z-direction motion. If zero, there is no motion in the z-coordinate system. Load curve ID defining the static coefficient of friction as a function of interface pressure. This option applies to shell segments only. Load curve ID defining the dynamic coefficient of friction as a function of interface pressure. This option applies to shell segments only. Scale factor on default slave penalty stiffness, see also *CON- TROL_CONTACT. Optional thickness for slave surface (overrides true thickness). This option applies to contact with shell, solid, and beam elements. True thickness is the element thickness of the shell elements. Thickness offsets are not used for solid element unless this option is specified. Scale factor for slave surface thickness (scales true thickness). This option applies only to contact with shell elements. True thickness is the element thickness of the shell elements. Contact surface maximum penetration check multiplier. If the penetration of a node through the rigid surface exceeds the product of XPENE and the slave node thickness, the node is set free. EQ.0: default is set to 4.0. Number of cycles between bucket sorts. The default value is set to 10 but can be much larger, e.g., 50-100, for fully connected surfaces. The contact formulation. The default, CTYPE = 0, is equivalent to the ONE_WAY_SURFACE_TO_SURFACE formulation, and CTYPE = 1 is a penalty formulation. If the slave surface belongs to a rigid body, CTYPE = 1 must be used. LCIDZ FSLCID FDLCID SFS STTHK SFTHK XPENE BSORT CTYPE Remarks: Thickness offsets do not apply to the rigid surface. There is no orientation requirement for the segments in the rigid surface, and the surface may be assembled from disjoint, but contiguous, arbitrarily oriented meshes. With disjoint meshes, the global searches must be done frequently, about every 10 cycles, to ensure a smooth movement of a slave node between mesh patches. For fully connected meshes this frequency interval can be safely set to 50-200 steps between searches. The modified binary database, d3plot, contains the road surface information prior to the state data. This information includes: NPDS = Total number of rigid surface points in problem. NRSC = Total number of rigid surface contact segments summed over all definitions. NSID = Number of rigid surface definitions. NVELQ = Number of words at the end of each binary output state defining the rigid surface motion. This equals 6 × NSID if any rigid surface moves or zero if all rigid surfaces are stationary. PIDS = An array equal in length to NPDS. This array defines the ID for each point in the road surface. XC = An array equal in length to 3 × NPDS. This array defines the global x, y, and z coordinates of each point. For each road surface define the following NSID sets of data: ID = Rigid surface ID. NS = Number of segments in rigid surface. IXRS = An array equal in length to 4 × NS. This is the connectivity of the rigid surface in the internal numbering system. At the end of each state, 6 × NVELQ words of information are written. For each road surface the x, y, and z displacements and velocities are written. If the road surface is fixed, a null vector should be output. Skip this section if NVELQ = 0. LS-PrePost currently displays rigid surfaces and animates their motion. *CONTACT Purpose: Define one-dimensional slide lines for rebar in concrete. Card 1 1 2 3 4 Variable NSIDS NSIDM ERR SIGC Type I I F Default none none 0. F 0. 5 GB F 0. 6 7 8 SMAX EXP F 0. F 0. VARIABLE DESCRIPTION NSIDS Nodal set ID for the slave nodes, see *SET_NODE. NSIDM Nodal set ID for the master nodes, see *SET_NODE. ERR SIGC GB External radius of rebar Unconfined compressive strength of concrete, 𝑓𝑐 Bond shear modulus SMAX Maximum shear strain EXP Exponent in damage curve Remarks: With this option the concrete is defined with solid elements and the rebar with truss elements, each with their own unique set of nodal points. A string of spatially consecutive nodes, called slave nodes, related to the truss elements may slide along another string of spatially consecutive nodes, called master nodes, related to the solid elements. The sliding commences after the rebar debonds. The bond between the rebar and concrete is assumed to be elastic perfectly plastic. The maximum allowable slip strain is given as: 𝑢max = SMAX × 𝑒−EXP×𝐷 where 𝐷 is the damage parameter 𝐷𝑛+1 = 𝐷𝑛 + Δ𝑢. The shear force, acting on area 𝐴𝑆, at time 𝑛 + 1 is given as: 𝑓𝑛+1 = min[𝑓𝑛 − GB × 𝐴𝑠 × Δ𝑢, GB × 𝐴𝑠 × 𝑢max] *CONTACT_2D_OPTION1_{OPTION2}_{OPTION3} Purpose: Define a 2-dimensional contact interface or slide line. This option is to be used with 2D solid and shell elements using the plane stress, plane strain or axisymmetric formulations, see *SECTION_SHELL and SECTION_BEAM. All the 2D contacts are supported in SMP. Only *CONTACT_2D_AUTOMATIC_SIN- GLE_SURFACE and *CONTACT_2D_AUTOMATIC_SURFACE_TO_SURFACE are supported for MPP. OPTION1 specifies the contact type. The following options activate kinematic constraints and should be used with deformable materials only, but may be used with rigid bodies if the rigid body is the master surface and all rigid body motions are prescribed. Kinematic constraints are recommended for high pressure hydrodynamic applications. SLIDING_ONLY TIED_SLIDING SLIDING_VOIDS AUTOMATIC_TIED_ONE_WAY The following option uses both kinematic constraints and penalty constraints. AUTOMATIC_TIED The following options are penalty based. These methods have no rigid-material limitations. They are recommended for lower pressure solid mechanics applications. PENALTY_FRICTION PENALTY AUTOMATIC_SINGLE_SURFACE AUTOMATIC_SINGLE_SURFACE_MORTAR AUTOMATIC_SURFACE_TO_SURFACE AUTOMATIC_SURFACE_TO_SURFACE_MORTAR AUTOMATIC_ONE_WAY_SURFACE_TO_SURFACE AUTOMATIC_SURFACE_IN_CONTINUUM For these contact types, the Mortar contact is available only for implicit and only supported in SMP at the moment. The following options are used for SPH particles in contact with 2D solid elements (2D shell elements are not supported currently) using the plane stress, plane strain or axisymmetric formulations: NODE_TO_SOLID NODE_TO_SOLID_TIED The following option is used to measure contact forces that are reported as RCFORC output. FORCE_TRANSDUCER OPTION2 specifies a thermal contact and takes the single option: THERMAL Only the AUTOMATIC contact options: SINGLE_SURFACE, SURFACE_TO_SUR- FACE, and ONE_WAY_SURFACE_TO_SURFACE may be used with the THERMAL option. OPTION3 specifies that the first card to read defines the title and ID number of contact interface and takes the single option: TITLE Title Card. Additional card for the TITLE keyword potion. Title 1 2 3 4 5 6 7 8 Variable CID Type I NAME A70 The 2D contact may be divided into 3 groups, each with a unique input format. 1. The first group were adopted from LS-DYNA2D and originated in the public domain version of DYNA2D from the Lawrence Livermore National Laborato- ry. Contact surfaces are specified as ordered sets of nodes. These sets define either contact surfaces or slide lines. The keyword options for the first group are: SLIDING_ONLY TIED_SLIDING SLIDING_VOIDS PENALTY_FRICTION PENALTY NOTE: TIED_SLIDING, PENALTY_FRICTION and PE- NALTY options are not recommended since there are automatic options in the second group that are easier to use and provide the same functionality. 2. The second group contains the automatic contacts. These contact surfaces may be defined using part sets or unordered node sets. Segment orientations are determined automatically. The keywords for these are: AUTOMATIC_SINGLE_SURFACE AUTOMATIC_SINGLE_SURFACE_MORTAR AUTOMATIC_SURFACE_TO_SURFACE AUTOMATIC_SURFACE_TO_SURFACE_MORTAR AUTOMATIC_ONE_WAY_SURFACE_TO_SURFACE AUTOMATIC_SURFACE_IN_CONTINUUM AUTOMATIC_TIED AUTOMATIC_TIED_ONE_WAY FORCE_TRANSDUCER 3. The third group is used for SPH particles in contact with continuum elements: NODE_TO_SOLID NODE_TO_SOLID_TIED Each of the 3 groups has a section below with a description of input and additional remarks. *CONTACT_2D_[SLIDING, TIED, & PENALTY]_OPTION This section documents the *CONTACT_2D variations derived from DYNA2D: SLIDING_ONLY TIED_SLIDING SLIDING_VOIDS PENALTY_FRICTION PENALTY. Card 1 1 2 3 4 5 6 7 8 Variable SSID MSID TBIRTH TDEATH Type I I F F Default none none 0. 1.e20 Card 2 1 2 3 4 5 6 7 8 Variable EXT_PAS THETA1 THETA2 TOL_IG PEN TOLOFF FRCSCL ONEWAY Type I F F F F F F F Default none none none 0.001 0.1 0.025 0.010 0.0 Friction Card. Additional card for the PENALTY_FRICTION keyword option. Card 3 1 2 3 4 5 6 7 8 Variable FRIC FRIC_L FRIC_H FRIC_S Type F F F VARIABLE SSID DESCRIPTION Nodal set ID for the slave nodes, see *SET_NODE. The slave surface must be to the left of the master surface. MSID Nodal set ID for the master nodes, see *SET_NODE. TBIRTH Birth time for contact. TDEATH Death time for contact. EXT_PAS Slide line extension bypass option. EQ.0: extensions are use EQ.1: extensions are not used THETA1 Angle in degrees of slide line extension at first master node. EQ.0: extension remains tangent to first master segment. THETA2 Angle in degrees of slide line extension at last master node. EQ.0: extension remains tangent to last master segment. TOL_IG Tolerance for determining initial gaps. EQ.0.0: default set to 0.001 PEN Scale factor or penalty. EQ.0.0: default set to 0.10 TOLOFF Tolerance for stiffness insertion for implicit solution only. The contact stiffness is inserted when a node approaches a segment a distance equal to the segment length multiplied by TOLOFF. The stiffness is increased as the node moves closer with the full stiffness being used when the nodal point finally makes contact. EQ.0.0: default set to 0.025. FRCSCL Scale factor for the interface friction. EQ.0.0: default set to 0.010 Better. This is the extensionwhen m17 is included. Poor. This is the extension if m17 is excluded from the slideline definition. This extension may spuriously interact with slave nodes s1 and s2. m9 m16 m15 m17 m1 m2 m3 m4 m5 m6m6 s1 s2 s3 s4 s5 s6 s7 s8 s9 s10 s15 s16 s17 s18 s19 s20 s21 s22 s23 m10 m11 m12 m13 s11 s12 s13 s14 s24 m7 m8 m14m14 Slide Lines 14 11 12 13 14 24 m s m s m s 17 24 23 22 21 20 19 18 17 16 15 14 13 12 11 19 15 16 10 11 Master Slide Line Slave Slide line Slide line Extension Master surface: nodes m1 - m17 Slave surface: nodes s1 - s24 Figure 11-26. Slide line Example. Note: (1) as recommend, for 90° angles each facet is assigned a distinct slide line; (2) the master slide line is more coarsely meshed; (3) the slave is to the left of the master (following the node ordering, see inset table); (4) as shown for slave nodes 1 and 2 it is important the slide line extension does not spuriously come into contact. VARIABLE ONEWAY DESCRIPTION Flag for one way treatment. If set to 1.0 the nodal points on the slave surface are constrained to the master surface. This option is generally recommended if the master surface is rigid. EQ.1.0: activate one way treatment. FRIC Coefficient of friction FRIC_L Coefficient of friction at low velocity. VARIABLE DESCRIPTION FRIC_H Coefficient of friction at high velocity. FRIC_S Friction factor for shear. Remarks: The SLIDING_ONLY option is a two-surface method based on a kinematic formulation. The two surfaces are allowed to slide arbitrarily large distances without friction, but are not permitted to separate or interpenetrate. Surfaces should be initially in contact. This option performs well when extremely high interface pressures are present. The more coarsely meshed surface should be chosen as the master surface for best performance. The TIED_SLIDING option joins two parts of a mesh with differing mesh refinement. It is a kinematic formulation so the more coarsely meshed surface should be chosen as the master. The SLIDING_VOIDS option is a kinematic formulation without friction which permits two surfaces to separate if tensile forces develop across the interface. The surfaces may be initially in contact or initially separated. The PENALTY_FRICTION and PENATLY options are penalty formulations so the designation of master and slave surfaces is not important. The two bodies may be initially separate or in contact. A rate-dependent Coulomb friction model is available for PENALTY_FRICTION. Consider two slide line surfaces in contact. It is necessary to designate one as a slave surface and the other as a master surface. Nodal points defining the slave surface are called slave nodes, and similarly, nodes defining the master surface are called master nodes. Each slave-master surface combination is referred to as a slide line. Many potential problems with the options can be avoided by observing the following precautions: • Metallic materials should contain the master surface along high explosive-metal interfaces. • SLIDING_ONLY type slide lines are appropriate along high explosive-metal interfaces. The penalty formulation is not recommended along such interfaces. • If one surface is more finely zoned, it should be used as the slave surface. If penalty slide lines are used, PENALTY and PENALTY_FRICTION, then the slave-master distinction is irrelevant. • A slave node may have more than one master segment, and may be included as a member of a master segment if a slide line intersection is defined. • Angles in the master side of a slide line that approach 90° must be avoided. Whenever such angles exist in a master surface, two or more slide lines should be defined. This procedure is illustrated in Figure 11-26. An exception for the foregoing rule arises if the surfaces are tied. In this case, only one slide line is needed. • Whenever two surfaces are in contact, the smaller of the two surfaces should be used as the slave surface. For example, in modeling a missile impacting a wall, the contact surface on the missile should be used as the slave surface. • Care should be used when defining a master surface to prevent the extension from interacting with the solution. In Figures 11-26 and 11-27, slide line exten- sions are shown. With extension of slide lines turned off, the slave nodes move down the inner walls as shown. Master surface Slave surface With extension and proper slide line definition, elements behave as expected. Slide line extension Extended slide lines do not allow for penetration Figure 11-27. With and without extension. Extensions may be turned off by setting EXT_PAS (card 2), but, when turned off, slave nodes may “leak” out as shown in the upper version of the figure. *CONTACT_2D_[AUTOMATIC, & FORCE_TRANSDUCER]_OPTION This section documents the following variations of *CONTACT_2D: AUTOMATIC_SINGLE_SURFACE AUTOMATIC_SINGLE_SURFACE_MORTAR AUTOMATIC_SURFACE_TO_SURFACE AUTOMATIC_SURFACE_TO_SURFACE_MORTAR AUTOMATIC_ONE_WAY_SURFACE_TO_SURFACE AUTOMATIC_SURFACE_IN_CONTINUUM AUTOMATIC_TIED AUTOMATIC_TIED_ONE_WAY FORCE_TRANSDUCER Card 1 1 2 3 4 Variable SIDS SIDM SFACT FREQ Type I I F I Default none none 1.0 50 8 5 FS F 0. 6 FD F 0. 7 DC F 0. Remarks 1 Card 2 1 1 2 3 4 5 6 7 8 Variable TBIRTH TDEATH SOS SOM NDS NDM COF INIT Type F F F F Default 0. 1.e20 1.0 1.0 Remarks 3 3 I 0 2 I 0 2 I 0 I 0 Automatic Thermal Card. Additional card for keywords with both the AUTOMATIC and THERMAL options. For example, *CONTACT_2D_AUTOMATIC_..._THERMAL_ ..... Card 3 Variable Type 1 K F 2 RAD F 3 H F 4 5 6 7 8 LMIN LMAX CHLM BC_FLAG Default none none none none none 1.0 F F F I 0 Automatic Optional Card 1. Optional card for the AUTOMATIC keyword option. Card 4 Variable 1 VC 2 3 4 5 6 7 8 VDC IPF SLIDE ISTIFF TIEDGAP IGAPCL TIETYP Type F F Default 0. 10.0 I 0 I 0 7 I 0 8 R 9 I 0 I 0 9 Remarks VARIABLE SIDS SIDM DESCRIPTION Set ID to define the slave surface. If SIDS > 0, a part set is assumed, see *SET_PART. If SIDS < 0, a node set with ID equal to the absolute value of SIDS is assumed, see *SET_NODE. Set ID to define the master surface. If SIDM > 0, a part set is assumed, see *SET_PART. If SIDM < 0, a node set with ID equal to the absolute value of SIDM is assumed, see *SET_NODE. Do not define for single surface contact. SFACT Scale factor for the penalty force stiffness. FREQ Search frequency. The number of timesteps between bucket sorts. For implicit contact this parameter is ignored and the search frequency is 1. FS FD EQ.0: default set to 50. Static coefficient of friction. The frictional coefficient is assumed to be dependent on the relative velocity 𝑣rel of the surfaces in contact according to the relation given by: 𝜇𝑐 = FD + (FS − FD)𝑒−DC∣𝑣𝑟𝑒𝑙∣. Dynamic coefficient of friction. The frictional coefficient is assumed to be dependent on the relative velocity 𝑣rel of the surfaces in contact 𝜇𝑐 = FD + (FS − FD)𝑒−DC∣𝑣rel∣. This parameter does not apply to Mortar contact. DC Exponential decay coefficient. The frictional coefficient is assumed to be dependent on the relative velocity 𝑣rel of the surfaces in contact 𝜇𝑐 = FD + (FS − FD)𝑒−DC∣𝑣rel∣. This parameter does not apply to Mortar contact. TBIRTH Birth time for contact. TDEATH Death time for contact. SOS Surface offset from midline for 2D shells of slave surface EQ.0.0: default to 1. GT.0.0: scale factor applied to actual thickness LT.0.0: absolute value is used as the offset SOM Surface offset from midline for 2D shells of master surface EQ.0: default to 1. GT.0: scale factor applied to actual thickness LT.0: absolute value is used as the offset NDS Normal direction flag for 2D shells of slave surface EQ.0: Normal direction is determined automatically EQ.1: Normal direction is in the positive direction EQ.-1: Normal direction is in the negative direction NDM Normal direction flag for 2D shells of master surface EQ.0: Normal direction is determined automatically EQ.1: Normal direction is in the positive direction EQ.-1: Normal direction is in the negative direction COF Closing/Opening flag for implicit contact EQ.0: Recommended for most problem where gaps are only closing. EQ.1: Recommended when gaps are opening to avoid sticking. This parameter does not apply to Mortar contact. INIT Special processing during initialization EQ.0: No special processing. EQ.1: Forming option. K RAD Thermal conductivity (k) of fluid between the slide surfaces. If a gap with a thickness 𝑙gap exists between the slide surfaces, then the conductance due to thermal conductivity between the slide surfaces is ℎcond = 𝑙gap Note that LS- DYNA calculates 𝑙gap based on deformation. Radiation factor, f, between the slide surfaces. A radiant-heat- transfer coefficient (ℎrad) is calculated . If a gap exists between the slide surfaces, then the contact conductance is calculated by ℎ = ℎcond + ℎrad H Heat transfer conductance (ℎ𝑐𝑜𝑛𝑡) for closed gaps. Use this heat transfer conductance for gaps in the range 0 ≤ 𝑙gap ≤ 𝑙min LMIN LMAX CHLM where 𝑙min is GCRIT defined below. Critical gap (𝑙min), use the heat transfer conductance defined (HTC) for gap thicknesses less than this value. No thermal contact if gap is greater than this value (𝑙max). Is a multiplier used on the element characteristic distance for the search routine. The characteristic length is the largest interface surface element diagonal. EQ.0: Default set to 1.0 BC_FLAG Thermal boundary condition flag EQ.0: thermal boundary conditions are on when parts are in contact EQ.1: thermal boundary conditions are off when parts are in contact VC Coefficient for viscous friction. This is used to limit the friction force to a maximum. A limiting force is computed 𝐹lim = VC × 𝐴cont. 𝐴cont being the area of contacted between segments. The suggested value for VC is to use the yield stress in shear: VC = 𝜎𝑜 √3 where 𝜎𝑜 is the yield stress of the contacted material. VDC Viscous damping coefficient in percent of critical for explicit contact. This parameter does not apply to Mortar contact. IPF Initial penetration flag for explicit contact. EQ.0: Allow initial penetrations to remain EQ.1: Push apart initially penetrated surfaces SLIDE Sliding option. EQ.0: Off EQ.1: On ISTIFF Stiffness scaling option. EQ.0: Use default option. EQ.1: Scale stiffness using segment masses and explicit time step (default for explicit contact) EQ.2: Scale stiffness using segment stiffness and dimensions (default for implicit contact) TIEDGAP Search gap for tied contacts. EQ.0: Default, use 1% of the master segment length GT.0: Use the input value LT.0: Use –TIEDGAP % of the master segment length. IGAPCL Flag to close gaps in tied contact EQ.0: Default, allow gaps to remain EQ.1: Move slave nodes to master segment to close gaps TIETYP Flag to control constraint type of tied contact EQ.0: Default, use kinematic constraints when possible EQ.1: Use only penalty type constraints Remarks: 1. The SINGLE_SURFACE, SURFACE_TO_SURFACE, and ONE_WAY_SUR- FACE_TO_SURFACE options use penalty forces to prevent penetration be- tween 2D shell elements and external faces of 2D continuum elements. Contact surfaces are defined using SIDS and SIDM to reference either part sets or node sets. If part sets are used, all elements and continuum faces of the parts in the set are included in contact. If node sets are used, elements or continuum faces that have both nodes in the set are included in the contact surface. The SIN- GLE_SURFACE option uses only the slave set and checks for contact between all elements and continuum faces in the set. If SSID is blank or zero, contact will be checked for all elements and continuum faces in the model. With the other options, both SSID and MSID are required. 2. The FORCE_TRANSDUCER option should be used in conjunction with at least one AUTOMATIC contact options. It does nothing to prevent penetration, but measures the forces generated by other contact definitions. The FORCE_- TRANSDUCER option uses only SIDS, and optionally SIDM. If only SIDS is defined, the force transducer measures the resultant contact force on all the elements and continuum faces in the slave surface. If both SIDS and SIDM are defined, then the force transducer measures contact forces between the ele- ments and continuum faces in the slave surface and master surface. The meas- ured forces are included in the rcforc output. In the case of an axisymmetric analysis, values output to rcforc and ncforc are in units of force per radian (this includes both shell types 14 and 15). 3. By default, the normal direction of 2D shell elements is evaluated automatically for SINGLE_SURFACE, SURFACE_TO_SURFACE and ONE_WAY_SUR- FACE_TO_SURFACE contact. The user can override the automatic algorithm using NDS or NDM and contact will occur with the positive or negative face of the element. 4. By default, the true thickness of 2D shell elements is taken into account for the SURFACE_TO_SURFACE, SINGLE_SURFACE, and ONE_WAY_SURFACE_- TO_SURFACE options. The user can override the true thickness by using SOS and SOM. If the surface offset is reduced to a small value, the automatic nor- mal direction algorithm may fail, so it is best to specify the normal direction using NDS or NDM. 5. For all AUTOMATIC contact options, eroding materials are treated by default. At present, subcycling is not possible. 6. The INIT parameter activates a forming option that is intended for implicit solutions of thin solid parts when back side segments may interfere with the solution. It automatically removes back side segments during initialization. Alternatively, the user can input INIT = 0, and use node set input to limit the contact interface to just the front of a thin part. 7. For the thermal option: ℎ = ℎcont, if the gap thickness is 0 ≤ 𝑙gap ≤ 𝑙min ℎ = ℎcond + ℎrad, if the gap thickness is 𝑙min ≤ 𝑙gap ≤ 𝑙max ℎ = 0, if the gap thickness is 𝑙gap > 𝑙max 8. The SLIDE parameter activates a sliding option which uses additional logic to improve sliding when surfaces in contact have kinks or corners. This option is off by default. 9. The ISTIFF option allows control of the equation used in calculating the penalty stiffness. For backward compatibility, the default values are different for im- plicit and explicit solutions. When ISTIFF = 1 is used, the explicit time step appears in the stiffness equation regardless if the calculation is implicit or ex- plicit. 10. The TIED_ONE_WAY contact creates two degree of freedom translational kinematic constraints to nodes on the slave surface which are initially located on or near master segments. The TIED option creates kinematic constraints between slave nodes and master segments, and also creates penalty constraints between master nodes and slave segments. With either contact option, a kine- matic constraint may be switched to penalty if there is a conflict with another constraint. The TIEDGAP parameter determines the maximum normal distance from a segment to a node for a constraint to be formed. Nodes will not be moved to eliminate an initial gap, and the initial gap will be maintained throughout the calculation. If TIETYP = 1, then only penalty constraints will be used. 11. Note that the SURFACE_IN_CONTINUUM option has been deprecated in favor of the *CONSTRAINED_LAGRANGE_IN_SOLID keyword which allows coupling between fluids and structures. However, this option is maintained to provide backward compatibility for existing data. For the SURFACE_IN_CONTINUUM option, penalty forces prevent the flow of slave element material (the continuum) through the master surfaces. Flow of the continuum tangent to the surface is permitted. Only 2D solid parts are permitted in the slave part set. Both 2D solid and 2D shell parts are permitted in the master part set. Flow through 2D shell elements is prevented in both directions by default. If NDM is set to ±1, flow in the direction of the normal is permitted. Thickness of 2D shell elements is ignored. 12. When using the SURFACE_IN_CONTINUUM option, there is no need to mesh the continuum around the structure because contact is not with continuum nodes but with material in the interior of the continuum elements. The algo- rithm works well for Eulerian or ALE elements since the structure does not interfere with remeshing. However, a structure will usually not penetrate the surface of an ALE continuum since the nodes are Lagrangian normal to the surface. Therefore, if using an ALE fluid, the structure should be initially im- mersed in the fluid and remain immersed throughout the calculation. Penetrat- ing the surface of an Eulerian continuum is not a problem. 13. The Mortar contact (MORTAR) is available for implicit calculations in SMP (MPP not supported). The apparent behavior compared to the non-Mortar contact is very similar, the difference lies in details concerning the constitutive relation (contact stress vs relative motion of contact surfaces) and the kinemat- ics (the relative motion of contact surfaces as function of nodal coordinates). Mortar contact is designed for continuity and smoothness that is beneficial for an implicit solution scheme, and is intended to enhance robustness in such a context. For details regarding the 2D Mortar contact, see the LS-DYNA Theory Manual. *CONTACT_2D_NODE_TO_SOLID_OPTION This section documents the following variations of *CONTACT_2D: NODE_TO_SOLID NODE_TO_SOLID_TIED Card 1 1 2 3 4 5 6 7 8 Variable SSID MSID TBIRTH TDEATH Type I I F F Default none None 0. 1.e20 3 VC F 4 5 OFFD PEN F F 6 FS F 7 FD F 8 DC F 0.0 0.0 1.0/0.1 0.0 0.0 0.0 Card 2 1 2 Variable SOFT Type Default I 0 VARIABLE SSID DESCRIPTION Nodal set ID or part set ID for the slave nodes, If SSID > 0, a nodal set ID is assumed, If SSID < 0 a part set ID is assumed. MSID Master part set ID. MSID < 0 since only part set is allowed. TBIRTH Birth time for contact. TDEATH Death time for contact. VARIABLE DESCRIPTION SOFT Soft constraint option: EQ.0: penalty formulation, EQ.1: soft constraint formulation. The soft constraint may be necessary if the material constants of the parts in contact have a wide variation in the elastic bulk moduli. In the soft constraint option, the interface stiffness is based on the nodal mass and the global time step size. The soft for axisymmetric is also recommended constraint option simulations. VC Coefficient for viscous friction. This is used to limit the friction force to a maximum. A limiting force is computed 𝐹lim = VC × 𝐴cont. 𝐴cont being the area of contacted between segments. The suggested value for VC is to use the yield stress in shear: VC = 𝜎𝑜 √3 where 𝜎𝑜 is the yield stress of the contacted material. OFFD Contact offset distance for slave nodes (SPH particles), not for tie contact right now. Recommended to be half of the original particle spacing in contact direction. PEN Scale factor for penalty. FS FD EQ.0.0: default set to 1.0 for penalty formulation, or 0.1 for soft constraint formulation. Static coefficient of friction. The frictional coefficient is assumed to be dependent on the relative velocity 𝑣rel of the surfaces in contact according to the relationship given by: 𝜇𝑐 = FD + (FS − FD)𝑒−DC∣𝑣rel∣. Dynamic coefficient of friction. The frictional coefficient is assumed to be dependent on the relative velocity 𝑣rel of the surfaces in contact 𝜇𝑐 = FD + (FS − FD)𝑒−DC∣𝑣rel∣. DESCRIPTION Exponential decay coefficient. The frictional coefficient is assumed to be dependent on the relative velocity vrel of the surfaces in contact 𝜇𝑐 = FD + (FS − FD)𝑒−DC∣𝑣rel∣. VARIABLE DC Remarks: NODE_TO_SOLID contact is a penalty based contact type used only for SPH particles with solid elements using the plane stress, plane strain or axisymmetric formulation. NODE_TO_SOLID_TIED contact is used only for SPH particles tied with solid elements, an offset of distance h (smooth length) is adopted for each SPH particle. The keyword control cards are optional and can be used to change defaults activate solution options such as mass scaling adaptive remeshing and an implicit solution however it is advisable to define the CONTROL_TERMINATION card. The ordering of the control cards in the input file is arbitrary. To avoid ambiguities define no more than one control card of each type. The following control cards are organized in alphabetical order *CONTROL_ACCURACY *CONTROL_ACOUSTIC *CONTROL_ADAPSTEP *CONTROL_ADAPTIVE *CONTROL_ADAPTIVE_CURVE *CONTROL_ALE *CONTROL_BULK_VISCOSITY *CONTROL_CHECK_SHELL *CONTROL_COARSEN *CONTROL_CONTACT *CONTROL_COUPLING *CONTROL_CPM *CONTROL_CPU *CONTROL_DEBUG *CONTROL_DISCRETE_ELEMENT *CONTROL_DYNAMIC_RELAXATION *CONTROL_EFG *CONTROL_ENERGY *CONTROL_EXPLICIT_THERMAL_ALE_COUPLING *CONTROL_EXPLICIT_THERMAL_BOUNDARY *CONTROL_EXPLICIT_THERMAL_INITIAL *CONTROL_EXPLICIT_THERMAL_OUTPUT *CONTROL_EXPLICIT_THERMAL_PROPERTIES *CONTROL_EXPLICIT_THERMAL_SOLVER *CONTROL_EXPLOSIVE_SHADOW *CONTROL_FORMING_AUTOCHECK *CONTROL_FORMING_AUTONET *CONTROL_FORMING_AUTOPOSITION_PARAMETER *CONTROL_FORMING_BESTFIT *CONTROL_FORMING_INITIAL_THICKNESS *CONTROL_FORMING_MAXID *CONTROL_FORMING_ONESTEP *CONTROL_FORMING_OUTPUT *CONTROL_FORMING_PARAMETER_READ *CONTROL_FORMING_POSITION *CONTROL_FORMING_PREBENDING *CONTROL_FORMING_PROJECTION *CONTROL_FORMING_REMOVE_ADAPTIVE_CONSTRAINTS *CONTROL_FORMING_SCRAP_FALL *CONTROL_FORMING_SHELL_TO_TSHELL *CONTROL_FORMING_STONING *CONTROL_FORMING_TEMPLATE *CONTROL_FORMING_TIPPING *CONTROL_FORMING_TOLERANC *CONTROL_FORMING_TRAVEL *CONTROL_FORMING_TRIMMING *CONTROL_FORMING_UNFLANGING *CONTROL_FORMING_USER *CONTROL_FREQUENCY_DOMAIN *CONTROL_HOURGLASS_{OPTION} *CONTROL_IMPLICIT_AUTO *CONTROL_IMPLICIT_BUCKLE *CONTROL_IMPLICIT_CONSISTENT_MASS *CONTROL_IMPLICIT_DYNAMICS *CONTROL_IMPLICIT_EIGENVALUE *CONTROL_IMPLICIT_FORMING *CONTROL_IMPLICIT_GENERAL *CONTROL_IMPLICIT_INERTIA_RELIEF *CONTROL_IMPLICIT_JOINTS *CONTROL_IMPLICIT_MODAL_DYNAMIC *CONTROL_IMPLICIT_MODAL_DYNAMIC_DAMPING_{OPTION} *CONTROL_IMPLICIT_MODAL_DYNAMIC_MODE_{OPTION} *CONTROL_IMPLICIT_MODES_{OPTION} *CONTROL_IMPLICIT_ROTATIONAL_DYNAMICS *CONTROL_IMPLICIT_SOLUTION *CONTROL_IMPLICIT_SOLVER *CONTROL_IMPLICIT_STABILIZATION *CONTROL_IMPLICIT_STATIC_CONDENSATION_{OPTION} *CONTROL_IMPLICIT_TERMINATION *CONTROL_MAT *CONTROL_MPP_DECOMPOSITION_ARRANGE_PARTS_{OPTION} *CONTROL_MPP_DECOMPOSITION_AUTOMATIC *CONTROL_MPP_DECOMPOSITION_BAGREF *CONTROL_MPP_DECOMPOSITION_CHECK_SPEED *CONTROL_MPP_DECOMPOSITION_CONTACT_DISTRIBUTE *CONTROL_MPP_DECOMPOSITION_CONTACT_ISOLATE *CONTROL_MPP_DECOMPOSITION_DISTRIBUTE_ALE_ELEMENTS *CONTROL_MPP_DECOMPOSITION_DISTRIBUTE_SPH_ELEMENTS *CONTROL_MPP_DECOMPOSITION_ELCOST *CONTROL_MPP_DECOMPOSITION_FILE *CONTROL_MPP_DECOMPOSITION_METHOD *CONTROL_MPP_DECOMPOSITION_NUMPROC *CONTROL_MPP_DECOMPOSITION_OUTDECOMP *CONTROL_MPP_DECOMPOSITION_PARTS_DISTRIBUTE *CONTROL_MPP_DECOMPOSITION_PARTSET_DISTRIBUTE_{OPTION} *CONTROL_MPP_DECOMPOSITION_RCBLOG *CONTROL_MPP_DECOMPOSITION_SCALE_CONTACT_COST *CONTROL_MPP_DECOMPOSITION_SCALE_FACTOR_SPH *CONTROL_MPP_DECOMPOSITION_SHOW *CONTROL_MPP_DECOMPOSITION_TRANSFORMATION *CONTROL_MPP_IO_BINOUTONLY *CONTROL_MPP_IO_LSTC_REDUCE *CONTROL_MPP_IO_NOBEAMOUT *CONTROL_MPP_IO_NOD3DUMP *CONTROL_MPP_IO_NODUMP *CONTROL_MPP_IO_NOFULL *CONTROL_MPP_IO_SWAPBYTES *CONTROL_MPP_MATERIAL_MODEL_DRIVER *CONTROL_MPP_PFILE *CONTROL_NONLOCAL *CONTROL_OUTPUT *CONTROL_PARALLEL *CONTROL_PORE_FLUID *CONTROL_REFINE_ALE *CONTROL_REFINE_ALE2D *CONTROL_REFINE_MPP_DISTRIBUTION *CONTROL_REFINE_SHELL *CONTROL_REFINE_SOLID *CONTROL_REMESHING *CONTROL_REQUIRE_REVISION *CONTROL_RIGID *CONTROL_SHELL *CONTROL_SOLID *CONTROL_SOLUTION *CONTROL_SPH *CONTROL_SPOTWELD_BEAM *CONTROL_START *CONTROL_STAGED_CONSTRUCTION *CONTROL_STEADY_STATE_ROLLING *CONTROL_STRUCTURED_{OPTION} *CONTROL_TERMINATION *CONTROL_THERMAL_EIGENVALUE *CONTROL_THERMAL_NONLINEAR *CONTROL_THERMAL_SOLVER *CONTROL_THERMAL_TIMESTEP *CONTROL_TIMESTEP *CONTROL_UNITS LS-DYNA’s implicit mode may be activated in two ways. Using the *CONTROL_IM- PLICIT_GENERAL keyword, a simulation may be flagged to run entirely in implicit mode. Alternatively, an explicit simulation may be seamlessly switched into implicit mode at the termination time using the *INTERFACE_SPRINGBACK_SEAMLESS keyword. The seamless switching feature is intended to simplify metal forming springback calculations, where the forming phase can be run in explicit mode, followed immediately by an implicit static springback simulation. In case of difficulty, restart capability is supported. Eight keywords are available to support implicit analysis. Default values are carefully selected to minimize input necessary for most simulations. These are summarized below: *CONTROL_IMPLICIT_GENERAL Activates implicit mode, selects time step size. *CONTROL_IMPLICIT_INERTIA_RELIEF Allows linear analysis of models with rigid body modes. *CONTROL_IMPLICIT_SOLVER Selects parameters for solving system of linear equations [K]{x}={f}. *CONTROL_IMPLICIT_SOLUTION Selects linear or nonlinear solution method, convergence tolerances. *CONTROL_IMPLICIT_AUTO Activates automatic time step control. *CONTROL_IMPLICIT_DYNAMICS Activates and controls dynamic implicit solution using Newmark method. *CONTROL_IMPLICIT_EIGENVALUE Activates and controls eigenvalue analysis. Activates and controls computation of constraint and attachment modes. *CONTROL_IMPLICIT_STABILIZATION Activates and controls artificial stabilization for multi-step spring back. *CONTROL_ACCURACY Purpose: Define control parameters that can improve the accuracy of the calculation. Card 1 1 2 3 4 5 6 7 8 Variable OSU INN PIDOSU IACC Type I I I I Default 0 (off) optional 0 (off) VARIABLE OSU DESCRIPTION Global flag for 2nd order objective stress updates . Generally, for explicit calculations only those parts undergoing large rotations, such as rolling tires, need this option. Objective stress updates can be activated for a subset of part IDs by defining the part set in columns 21-30. EQ.0: Off (default) EQ.1: On INN Invariant node numbering for shell and solid elements. . EQ.-4: On for both shell and solid elements except triangular shells EQ.-2: On for shell elements except triangular shells EQ.1: Off (default for explicit) EQ.2: On for shell and thick shell elements (default for implicit) EQ.3: On for solid elements EQ.4: On for shell, thick shell, and solid elements PIDOSU Part set ID for objective stress updates. If this part set ID is given only those part IDs listed will use the objective stress update; therefore, OSU is ignored. DESCRIPTION Implicit accuracy turns on some specific accuracy considerations in implicit analysis at an extra CPU cost. See Remark 4. flag, EQ.0: Off (default) EQ.1: On VARIABLE IACC Remarks: 1. Second Order Objective Stress Update. Second order objective stress updates are occasionally necessary. Some examples include spinning bodies such as turbine blades in a jet engine, high velocity impacts generating large strains in a few time steps, and large time step sizes due to mass scaling in metal forming. There is a significantly added cost which is due in part to the added cost of the second order terms in the stress update when the Jaumann rate is used and the need to compute the strain-displacement matrix at the mid- point geometry. This option is available for one point brick elements, the selec- tive-reduced integrated brick element which uses eight integration points, the fully integrated plane strain and axisymmetric volume weighted (type 15) 2D solid elements, the thick shell elements, and the following shell elements: Be- lytschko-Tsay, Belytschko-Tsay with warping stiffness, Belytschko-Chiang- Wong, S/R Hughes-Liu, and the type 16 fully integrated shell element. 2. Invariant Node Numbering for Shell Elements. Invariant node numbering for shell and thick shell elements affects the choice of the local element shell coordinate system. The orientation of the default local coordinate system is based on the shell normal vector and the direction of the 1-2 side of the element. If the element numbering is permuted, the results will change in irregularly shaped elements. With invariant node numbering, permuting the nodes shifts the local system by an exact multiple of 90 degrees. In spite of its higher costs [<5%], the invariant local system is recommended for several reasons. First, element forces are nearly independent of node sequencing; secondly, the hour- glass modes will not substantially affect the material directions; and, finally, stable calculations over long time periods are achievable. The INN parameter has no effect on thick shell form 2 which is always invariant and thick shell from 3 which is never invariant. 3. Invariant Node Numbering for Solid Elements. Invariant node numbering for solid elements is available for anisotropic materials only. This option has no effect on solid elements of isotropic material. This option is recommended when solid elements of anisotropic material undergo significant deformation. 4. Implicit Calculations. All other things being equal, a single time step of an implicit analysis usually involves a larger time increment and deformation than an explicit analysis. Many of the algorithms in LS-DYNA have been heavily optimized for explicit analysis in ways that are inappropriate for implicit analy- sis. While an implicit analysis, by default, invokes many measures to ensure accuracy, certain corrections associated with unusual applications or with large computational expense are invoked only by setting IACC = 1. A list of features that are included with this option follows. a) Strongly objective treatment of some tied contact interfaces, see *CONTACT. b) Fully iterative treatment of some piecewise linear plasticity materials, see *MAT_PIECEWISE_LINEAR_PLASTICITY *MAT_MODIFIED_- PIECEWISE_LINEAR_PLASTICITY, including smooth decay of stresses down to zero when including failure. and c) Strong objective treatment of some elements in the context of large rota- tions, applies to shell element types -16, 16 and 4, beam element types 1, 2 and 9, and solid element types -2, -1, 1, 2 and 16. The superposed rigid body motion is subtracted from these elements before evaluating the re- sponse which significantly reduces the presence of spurious strains. *CONTROL Purpose: Define control parameters for transient acoustic solutions. Card 1 1 2 3 4 5 6 7 8 Variable MACDVP Type Default I 0 VARIABLE MACDVP Remarks: DESCRIPTION Calculate the nodal displacements and velocities of *MAT_- ACOUSTIC volume elements for inclusion in d3plot and time- history files. EQ.0: Acoustic nodal motions will not be calculated EQ.1: Acoustic nodal motions will be calculated 1. *MAT_ACOUSTIC volume elements (ELFORM = 8 and ELFORM = 14) use the displacement potential as the fundamental unknown. The infinitesimal mo- tions of these acoustic nodes can be found from the gradient of the displace- ment and velocity potentials. This is purely a post-processing endeavor and has no effect on the predicted pressures and structural response. It will howev- er roughly double the cost of the acoustic solution and for that reason is not done by default. 2. The acoustic theory underpinning *MAT_ACOUSTIC volume elements presumes infinitesimal motions. In the presence of larger motions the pressure calculations will proceed regardless, but the calculation of acoustic nodal mo- tions can then be unreliable. *CONTROL_ADAPSTEP Purpose: Define control parameters for contact interface force update during each adaptive cycle. Card 1 1 2 3 4 5 6 7 8 Variable FACTIN DFACTR Type F F Default 1.0 0.01 VARIABLE FACTIN DESCRIPTION Initial relaxation factor for contact force during each adaptive remesh. To turn this option off set FACTIN = 1.0. Unless stability problems occur in the contact, FACTIN = 1.0 is recommended since this option can create some numerical noise in the resultant tooling forces. A typical value for this parameter is 0.10. DFACTR Incremental increase of FACTIN during each time step after the adaptive step. FACTIN is not allowed to exceed unity. A typical value might be 0.01. Remarks: 1. This command applies to contact with thickness offsets including contact types: *CONTACT_FORMING_…_ *CONTACT_NODES_TO_SURFACE_ *CONTACT_SURFACE_TO_SURFACE *CONTACT_ONE_WAY_SURFACE_TO_SURFACE. *CONTROL Purpose: Activate adaptive meshing. The parts which are adaptively meshed are defined by ADPOPT under *PART. Note that “sandwiched” part’s adaptivity is available when the variable IFSAND is set to “1” and applies to ADPOPT = 1 and 2 only. Other related keywords include: *CONTROL_ADAPTIVE_CURVE, *DEFINE_- CURVE_TRIM (with variable TCTOL), *DEFINE_BOX_ADAPTIVE (moving adaptive box), and *DEFINE_CURVE_BOX_ADAPTIVITY. This keword is applicable to neither hyperelastic materials nor any material model based on a Total Lagrangian formulation. Card 1 1 2 3 4 5 6 7 8 Variable ADPFREQ ADPTOL ADPOPT MAXLVL TBIRTH TDEATH LCADP IOFLAG Type F F Default none 1020 I 1 I 3 F F 0.0 1020 I 0 I 0 Remaining cards are optional.† Card 2 1 2 3 4 5 6 7 8 Variable ADPSIZE ADPASS IREFLG ADPENE ADPTH MEMORY ORIENT MAXEL Type F Default Card 3 1 I 0 2 I 0 3 F F I I I 0.0 inactive inactive 0 inactive 4 5 6 7 8 Variable IADPN90 IADPGH NCFREQ IADPCL ADPCTL CBIRTH CDEATH LCLVL Type Default I 0 I 0 I none I 1 F F F F none 0.0 1020 Card 4 1 2 3 4 5 6 7 8 Variable CNLA MMM2D ADPERR D3TRACE IFSAND Type Default F 0 VARIABLE ADPFREQ ADPTOL I 0 I 0 I 0 I 0 DESCRIPTION Time interval between adaptive refinements, see Figures 12-2 and 12-1. Adaptive error tolerance in degrees for ADPOPT set to 1 or 2 below. If ADPOPT is set to 8, ADPTOL is the characteristic element size. ADPOPT Adaptive options: EQ.1: angle change in degrees per adaptive refinement relative to the surrounding shells for each shell to be refined. EQ.2: total angle change in degrees relative to the surrounding shells for each shell to be refined. For example, if the adptol = 5 degrees, the shell will be refined to the second level when the total angle change reaches 5 degrees. When the angle change is 10 degrees the shell will be refined to the third level. EQ.4: adapts when the shell error in the energy norm, Δ𝑒, exceeds ADPTOL/100 times the mean energy norm within the part, which is estimated as: Δ𝑒 = (∫ Ω𝑒 2⁄ ‖Δ𝜎‖2 𝑑Ω ) where 𝐸 is Young's modulus. The error of the stresses Δ𝜎 is defined as the difference between the the recovered solution 𝜎 ⋆ and i.e. Δ𝜎 ≡ 𝜎 ⋆ − 𝜎 ℎ. Various recovery techniques for 𝜎 ⋆ and error estimators for Δ𝑒 are defined by ADPERR. This options works for shell types 2, 4, 16, 18, 20. the numerical solution, 𝜎 ℎ EQ.7: 3D r-adaptive remeshing for solid elements. Solid element type 13, a tetrahedron, and 3-D EFG type 41 and 42, are used in the adaptive remeshing process. A com- VARIABLE DESCRIPTION pletely new mesh is generated which is initialized from the old mesh using a least squares approximation. The mesh size is currently based on the minimum and maxi- mum edge the *CONTROL_- REMESHING keyword input. This option remains under development, and, we are not sure of its reliability on complex geometries. lengths defined on EQ.8: 2D 𝑟-adaptive remeshing for axisymmetric and plane strain continuum elements. A completely new mesh is generated which is initialized from the old mesh using a least squares approximation. The mesh size is currently based on the value, ADPTOL, which gives the character- istic element size. This option is based on earlier work by Dick and Harris [1992]. If ADPTOL is negative, then self-contacting material will not be merged together. The self-merging is often preferred since it eliminates sharp folds in the boundary; however, if the sharp fold is being simulated unexpected results are generated. Maximum number of refinement levels. Values of 1, 2, 3, 4, … allow a maximum of 1, 4, 16, 64, … shells, respectively, to be created for each original shell. The refinement level can be overridden by *DEFINE_BOX_ADAPTIVE, or *DEFINE_SET_- ADAPTIVE. Birth time at which the adaptive remeshing begins, see Figures 12-2 and 12-1. Death time at which the adaptive remeshing ends, see Figures 12-2 and 12-1. Adaptive interval is changed as a function of time given by load curve ID, LCADP. If this option is nonzero, the ADPFREQ will be replaced by LCADP. The 𝑥-axis is time and the 𝑦-axis is the varied adaptive time interval. Flag to generate adaptive mesh at exit including *NODE, *ELE- MENT_SHELL_THICKNESS, *BOUNDARY_option, and *CON- STRAINED_ADAPTIVITY, to be saved in the file, adapt.msh. EQ.1: generate ℎ-adapted mesh. MAXLVL TBIRTH TDEATH LCADP IOFLAG ADPSIZE Minimum shell size to be adapted based on element edge length. If undefined the edge length limit is ignored. (cid:98)(cid:106)(cid:29)(cid:97)(cid:106)(cid:89) (cid:70)(cid:51)(cid:51)(cid:85) (cid:106)(cid:67)(cid:76)(cid:51) (cid:64)(cid:67)(cid:99)(cid:65) (cid:106)(cid:82)(cid:97)(cid:119) (cid:67)(cid:78) (cid:47)(cid:107)(cid:84)(cid:72)(cid:81)(cid:105)(cid:89) (cid:50)(cid:113)(cid:82)(cid:73)(cid:113)(cid:51) (cid:56)(cid:97)(cid:82)(cid:76) (cid:486) (cid:106)(cid:82) (cid:486)(cid:3718) (cid:30) (cid:486) (cid:12) (cid:34)(cid:37)(cid:49)(cid:39)(cid:51)(cid:38)(cid:50)(cid:15) (cid:99)(cid:51)(cid:106)(cid:45) (cid:486) (cid:30) (cid:486)(cid:3718) (cid:106)(cid:51)(cid:97)(cid:67)(cid:76)(cid:67)(cid:78)(cid:29)(cid:106)(cid:67)(cid:82)(cid:78) (cid:106)(cid:67)(cid:76)(cid:51) (cid:97)(cid:51)(cid:29)(cid:44)(cid:64)(cid:51)(cid:48)(cid:93) (cid:119)(cid:51)(cid:99) (cid:50)(cid:113)(cid:82)(cid:73)(cid:113)(cid:51) (cid:56)(cid:97)(cid:82)(cid:76) (cid:486) (cid:106)(cid:82) (cid:486)(cid:3718) (cid:82)(cid:78) (cid:97)(cid:51)(cid:126)(cid:78)(cid:51)(cid:48) (cid:76)(cid:51)(cid:99)(cid:64)(cid:89) (cid:105)(cid:51)(cid:97)(cid:76)(cid:67)(cid:78)(cid:29)(cid:106)(cid:51)(cid:89) (cid:114)(cid:97)(cid:67)(cid:106)(cid:51) (cid:106)(cid:82) (cid:47)(cid:107)(cid:84)(cid:72)(cid:81)(cid:105)(cid:89) (cid:78)(cid:82) (cid:70)(cid:83)(cid:83)(cid:80)(cid:83) (cid:29) (cid:85)(cid:80)(cid:77)(cid:70)(cid:83)(cid:66)(cid:79)(cid:68)(cid:70)(cid:93) (cid:78)(cid:82) (cid:96)(cid:51)(cid:126)(cid:78)(cid:51) (cid:76)(cid:51)(cid:99)(cid:64) (cid:29)(cid:106) (cid:106)(cid:67)(cid:76)(cid:51) (cid:486) (cid:86)(cid:78)(cid:82)(cid:106) (cid:486)(cid:3718)(cid:87)(cid:89) (cid:47)(cid:82)(cid:78)(cid:533)(cid:106) (cid:99)(cid:29)(cid:113)(cid:51) (cid:110)(cid:78)(cid:97)(cid:51)(cid:126)(cid:78)(cid:51)(cid:48) (cid:99)(cid:82)(cid:73)(cid:110)(cid:106)(cid:67)(cid:82)(cid:78)(cid:89) (cid:119)(cid:51)(cid:99) (cid:99)(cid:51)(cid:106)(cid:45) (cid:486) (cid:30) (cid:486)(cid:3718) write re(cid:1)ne time 22 tbirth 11 33 ADPFREQ end time Figure 12-1. Flowchart for ADPASS = 0. While this option is sometimes more accurate, ADPASS = 1 is much less expensive and recommended when used with ADPENE. VARIABLE DESCRIPTION LT.0: absolute value defines the minimum characteristic element length to be adapted based on square root of the element area, i.e., instead of comparing the shortest ele- ment edge with ADPSIZE, it compares the square root of the element area with |ADPSIZE| whenever ADPSIZE is defined by a negative value. ADPASS One or two pass flag for ℎ-adaptivity: EQ.0: two pass adaptivity as shown in Figure 12-2. EQ.1: one pass adaptivity as shown in Figure 12-1. IREFLG Uniform refinement level. A value of 1, 2, 3 … allow 4, 16, 64 … shells, respectively, to be created uniformly for each original shell. If negative, |IREFLG| is taken as a load curve ID. With the curve time tbirth (cid:98)(cid:106)(cid:29)(cid:97)(cid:106)(cid:89) (cid:70)(cid:51)(cid:51)(cid:85) (cid:106)(cid:67)(cid:76)(cid:51) (cid:64)(cid:67)(cid:99)(cid:65) (cid:106)(cid:82)(cid:97)(cid:119) (cid:67)(cid:78) (cid:47)(cid:107)(cid:84)(cid:72)(cid:81)(cid:105)(cid:89) (cid:51)(cid:113)(cid:82)(cid:73)(cid:113)(cid:51) (cid:106)(cid:67)(cid:76)(cid:51) (cid:106)(cid:82) (cid:486) (cid:12) (cid:34)(cid:37)(cid:49)(cid:39)(cid:51)(cid:38)(cid:50) ADPFREQ (cid:119)(cid:51)(cid:99) (cid:105)(cid:51)(cid:97)(cid:76)(cid:67)(cid:78)(cid:29)(cid:106)(cid:51)(cid:89) (cid:114)(cid:97)(cid:67)(cid:106)(cid:51) (cid:106)(cid:82) (cid:47)(cid:107)(cid:84)(cid:72)(cid:81)(cid:105)(cid:89) (cid:106)(cid:51)(cid:97)(cid:67)(cid:76)(cid:67)(cid:78)(cid:29)(cid:106)(cid:67)(cid:82)(cid:78) (cid:106)(cid:67)(cid:76)(cid:51) (cid:97)(cid:51)(cid:29)(cid:44)(cid:64)(cid:51)(cid:48)(cid:93) (cid:78)(cid:82) (cid:97)(cid:51)(cid:126)(cid:78)(cid:51) (cid:76)(cid:51)(cid:99)(cid:64)(cid:46) (cid:67)(cid:56) (cid:97)(cid:51)(cid:92)(cid:110)(cid:67)(cid:97)(cid:51)(cid:48) re(cid:1)ne re(cid:1)ne re(cid:1)ne re(cid:1)ne end time Figure 12-2. Flow chart for ADPASS = 1. This algorithm may be summarized as, “periodically refine” This method is recommended over ADPASS = 0 when used with ADPENE, which implements look ahead. VARIABLE DESCRIPTION option, the abscissa values define the refinement time, and the ordinate values define the minimum element size. Only one refinement level is performed per time step. An advantage of the load curve option is that the mesh is adapted to honor the minimum element size, but with the uniform option, IREFLG > 0, this is not possible. NOTE: If the element size defined with *DEFINE_CURVE is positive, the element size will override the element size defined with *CONTROL_ADAPTIVE and *DEFINE_SET_ADAPTIVE. Also, if the element size defined with *DEFINE_CURVE is negative the element size is used for refinement only. For shell, ℎ-adapt the mesh when the FORMING contact surfaces approach or penetrate the tooling surface depending on whether is positive (approach) or negative the value of ADPENE (penetrates), respectively. The tooling adaptive refinement is based on the curvature of the tooling. If ADPENE is positive the takes place; refinement generally occurs before contact ADPENE VARIABLE DESCRIPTION consequently, it is possible that the parameter ADPASS can be set to 1 in invoke the one pass adaptivity. For three dimensions 𝑟-adaptive solid remeshing (ADPOPT = 2 in *PART), the mesh refinement is based on the curvature of the tooling when ADPENE is positive. See Remark 6. ADPTH EQ.0.0: This parameter is ignored GT.0.0: Absolute shell thickness level below which adaptive remeshing should began. LT.0.0: Element thickness reduction ratio. If the ratio of the element thickness to the original element thickness is less than 1.0+ADPTHK, the element will be refined. This option works only if ADPTOL is nonzero. If thickness based adaptive remeshing is desired without angle changes, then, set ADPTOL to a large angle. MEMORY the machine and operating system This flag can have two meanings depending on whether the memory environmental variable is or is not set. The command "setenv LSTC_MEMORY auto" (or for bourne shell “export LSTC_MEMORY=auto”) sets the memory environmental variable which causes LS-DYNA to expand memory automatically. Note that automatic memory expansion is not always 100% reliable depending on level; consequently, it is not yet the default. To see if this is set on a particular machine type the command "env". If the environmen- tal variable is not set then when memory usage reaches this percentage, MEMORY, further adaptivity is prevented to avoid exceeding the memory specified at execution time. Caution is necessary since memory usage is checked after each adaptive step, and, if the memory usage increases by more than the residual percentage, 100-PERCENT, calculation will terminate. If the memory environmental variable is set then when the number of words of memory allocated reaches or exceeds this value, MEMORY, further adaptivity is stopped. the ORIENT This option applies to the FORMING contact option only. If this flag is set to one (1), the user orientation for the contact interface is used. If this flag is set to zero (0), LS-DYNA sets the global orientation of the contact surface the first time a potential contact is observed after the birth time. If slave nodes are found on both sides of the contact surface, the orientation is set based on the VARIABLE DESCRIPTION principle of "majority rules". Experience has shown that this principle is not always reliable. MAXEL Adaptivity is stopped if this number of shells is exceeded. IADPN90 Maximum number of shells covering 90 degree of radii. See Remark 5. IADPGH Fission flag for neighbor splitting. EQ.0: split all neighbor shells EQ.1: do not split neighbor shells NCFREQ IADPCL ADPCTL CBIRTH Frequency of fission to fusion steps. For example, if NCFREQ = 4, then fusion will occur on the fourth, eighth, twelfth, etc., fission steps, respectively. If this option is used NCFREQ > 1 is recommended. Fusion will not occur until the fission level reaches IADPCL. Therefore, if IADPCL = 2, MAXLVL = 5, any shell can be split into 256 shells. If the surface flattens out, the number of elements will be reduced if the fusion option is active, i.e., the 256 elements can be fused and reduced to 16. Adaptivity error tolerance in degrees for activating fusion. It follows the same rules as ADPOPT above. Birth time for adaptive fusion. If ADPENE > 0, look-ahead adaptivity is active. In this case, fission, based on local tool curvature, will occur while the blank is still relatively flat. The time value given for CBIRTH should be set to a time later in the simulation after the forming process is well underway. CDEATH Death time for adaptive fusion. LCLVL Load curve ID of a curve that defines the maximum refinement level as a function of time CNLA Limit angle for corner nodes. See Remark 7. MMM2D ADPERR If non-zero, common boundaries of all adapted materials will be merged. Only for 2D r-adaptivity 3-digit number, as “𝑋𝑌𝑌”, where “𝑋” and “𝑌𝑌” define the options for the recovery techniques and the error estimators, VARIABLE DESCRIPTION respectively, For 𝑋: EQ.0: superconvergent patch recovery (SPR) (default); EQ.1: the least square fit of the stress to the nodes (Global L2); EQ.2: error density SPR, as Δ𝑒 ̃ = Δ𝑒/Areaelement; EQ.3: self-weighted SPR, as Δ𝑒 ̊ = √Δ𝑒 × 𝑒 For 𝑌𝑌: EQ.00: energy norm (default) EQ.01: Cauchy 𝜎𝑥 EQ.02: 𝜎𝑦 EQ.03: 𝜎𝑧 EQ.04: 𝜏𝑥𝑦 EQ.05: 𝜏𝑦𝑧 EQ.06: 𝜏𝑧𝑥 EQ.07: effective plastic strain, 𝜀ep EQ.08: pressure EQ.09: von Mises EQ.10: principal deviator stress s11 EQ.11: 𝑆22 EQ.12: 𝑆33 EQ.13: Tresca EQ.14: principal stress 𝜎11 EQ.15: 𝜎22 EQ.16: 𝜎33 EQ.20: user subroutine “uadpval” to extract the numerical solutions for recovery, and “uadpnorm” to provide an error estimator. D3TRACE Flag that is either 0 or 1. If set to 1 then a d3plot state will be output just before and after an adaptive step even though it may not be requested. The reason for wanting to do this is to allow the LS-PrePost particle trace algorithm to work in the case of VARIABLE DESCRIPTION adaptivity. IFSAND Set this flag to “1” for forming of sandwiched parts with adaptive blank mesh, see Remarks. Currently the adaptivity is limited to only one layer of solid element, and applies to ADPOPT = 1 and 2 only. Remarks about 3D adaptivity: 1. Restarting. The d3dump and runrsf files contain all information necessary to restart an adaptive run. This did not work in version 936 of LS-DYNA. 2. Related Field in *PART. In order for this control card to work, the flag ADPOPT=1 must be set in the *PART definition. Otherwise, adaptivity will not function. 3. Contact Types and Options. In order for adaptivity to work optimally, the parameter SNLOG=1, must be set on Optional Control Card B in the *CON- TACT Section. On disjoint tooling meshes the contact option *CONTACT_- FORMING_… is recommended. 4. Root ID (RID) File. A file named “adapt.rid” is left on disk after the adaptive run is completed. This file contains the root ID of all elements that are created during the calculation, and it does not need to be kept if it is not used in post- processing. 5. Note About IADPN90 Field. For all metal forming simulation, IADPN90 should be set to -1. 6. Contact and ADPENE. In three dimensions when ADPENE>0 it is presumed that the solid part to be adapted is on the slave side of a contact, and the “tool- ing”, consisting of a shell surface, is on the master side of that same contact. ADPENE>0 represents a distance from the tooling surface within which the adapted mesh refinement of the slave part is influenced by the radius of curva- ture of the tooling surface. This feature is currently unavailable in SMP and SOFT=2 in *CONTACT. Remarks about 2D r-adaptivity: 7. CNLA Field. In two dimensions 𝑟-adaptive remeshing, the generated new mesh should have a node at each corner so that corners are not smoothed. By default, the mesher will assume a corner wherever the interior angel between adjacent edges is less than 110 degrees. Setting CNLA larger than 110 enables angles larger than 110 to be corners. Care should be taken to avoid an unneces- sarily large value of CNLA as this may prevent the mesher from generating smooth meshes. Remarks about mesh adaptivity for sandwiched parts (IFSAND): 8. Sandwiched parts (also called laminates) consist layers of solid elements (core) sandwiched by one layer of shell elements each on top and bottom surface of the solid elements, as shown in Figure 12-3. Common nodes are used for solid and shell interface. Currently mesh adaptivity is limited to only one layer of solid element with mesh refinements in-plane on both solids and shells. Note sandwiched parts can be trimmed by setting ITYP = 1 in keyword keyword *CONTROL_FORMING_TRIMMING *DEFINE_CURVE_TRIM. Trimming of sandwiched parts allows for multiple layers of solids. with and In a typical forming set up, the following cards need to be changed to activate the sandwiched part mesh adaptivity: *CONTROL_ADAPTIVE $# adpfreq adptol adpopt maxlvl tbirth tdeath lcadp ioflag &adpfq 4.0000E+00 1 4 0.0001.0000E+20 0 0 $# adpsize adpass ireflg adpene adpth memory orient maxel 0.90000 1 10.00000 0.000 0 0 0 $# ladpn90 ladpgh ncfred ladpcl adpctl cbirth cdeath lclvl -1 0 0 1 0.000 0.0001.0000E+20 0 $ IFSAND 1 *PART Mid-core layer of solid elements $ PID SECID MID EOSID HGID GRAV ADPOPT TMID 1 1 1 1 Top layer of shell elements 100 100 1 1 Bottom layer of shell elements 101 100 1 1 Note IFSAND in *CONTROL_ADAPTIVE is set to “1” to activate the sandwich part adaptivity; ADPOPT under *PART are all set to “1” to activate the adaptivity. Revision Information: 9. IFSAND is available starting in Rev 104365 in both SMP and MPP versions. Later revisions may include improvements. layer of Top shell elements Only 1 layer of 3-D solid elements are allowed Bottom layer of shell elements Figure 12-3. Mesh adaptivity of sandwiched parts (IFSAND). *CONTROL_ADAPTIVE_CURVE Purpose: To refine the element mesh along a curve during or prior to sheet metal forming simulation. All curves defined by the keyword *DEFINE_CURVE_TRIM are used in the refinement. This option provides additional refinement to that created by *CONTROL_ADAPTIVE. Additionally, pre-mesh refinement along a curve with specific distance/range on both sides of the curve can be modeled when this keyword is used together with *DEFINE_CURVE_TRIM_3D (by activating the variable TCTOL). Lastly, the keyword can be used to refine mesh along a curve during trimming when used together with the keyword *ELEMENT_TRIM. This feature only applies to shell elements. Card 1 1 2 Variable IDSET ITYPE Type I I 3 N I 4 5 6 7 8 SMIN ITRIOPT F I VARIABLE DESCRIPTION IDSET ITYPE Set ID Set type: EQ.1: IDSET is shell set ID. EQ.2: IDSET is part set ID. N Refinement option: EQ.1: Refine until there are no adaptive constraints remaining in the element mesh around the curve, subjected to the maximum refinement level of 5. GT.1: Refine no more than N levels. SMIN If the element dimension is smaller than this value, do not refine. ITRIOPT Option to refine an enclosed area of a trim curve. EQ.0: Refine the elements along the trim curve. EQ.1: Refine the elements along the trim curve and enclosed by the trim curve. Adaptive mesh refinement along a curve during a simulation: In Figure 12-4, an example is shown to illustrate the mesh adaptivity along an enclosed curve. Since the mesh refinement is controlled by the refinement level “N” and smallest element size “SMIN”, care should be taken so not too many elements are generated during the run. A partial input example is listed below, where mesh will be refined by four levels, or to no smaller than 0.3mm element edge length, along both sides of the curve defined by IGES format file “adpcurves.iges”. *INCLUDE drawn.dynain *DEFINE_CURVE_TRIM_3D $ TCID TCTYPE TFLG TDIR TCTOL 1 2 adpcurves.iges *CONTROL_ADAPTIVE_CURVE $ IDSET ITYPE N SMIN 1 2 4 0.3 Since this method tends to create too many elements during refinement, the following feature was added to address the issue. Adaptive mesh refinement along a curve in the beginning of a simulation: When TCTOL is defined under the keyword *DEFINE_CURVE_TRIM_3D, it is used as a distance definition, and together with *CONTROL_ADAPTIVE_CURVE, the mesh will be refined in the beginning of a (flanging, etc.) simulation, along both sides of the defined curve, limited within the distance specified, as shown in Figures 12-5 and 12-6. In addition, this feature works with the option 3D only. It is noted that the curve needs to be sufficient close to the part, and this can be accomplished in LS-PrePost4.0 under GeoTol/Project/Closest Proj/Project to Element/By Part. Furthermore, since the curve is often made from some feature lines of forming tools, it is important the curve is re- positioned closer to the blank, or better yet, is projected onto the blank; otherwise the refinement will not take place. A partial input example is listed below, where mesh will be refined within a range of 4.0mm, formed by 2.0mm distance (TCTOL = 2.0) of both sides of the curve, defined by file “adpcurves.iges”. The maximum refine level is 4 and minimum element size allowed is 0.3mm. *INCLUDE drawn.dynain *DEFINE_CURVE_TRIM_3D $ TCID TCTYPE TFLG TDIR TCTOL 1 2 0 0 2.000 adpcurves.iges *CONTROL_ADAPTIVE_CURVE $ IDSET ITYPE N SMIN 1 2 4 0.3 Mesh refinement along a curve is very useful during line die simulation. For example, in a flanging simulation, a trimmed blank, where it is mostly flat in the flanging break line in draw die, can be refined using a curve generated from the trim post radius. In LS-PrePost 4.0, the curve can be generated using Curve/Spline/From Mesh/By Edge, check Prop, and defining a large Ang to create a continuous curve along element edge. This curve can then be projected onto the blank mesh using GeoTol/Project feature, to be used as the curve file “adpcurves.iges” here. The mesh pre-refinement along curves are implemented in ‘flanging’ process starting in LS-PrePost4.0 eZSetup for metal forming application. In LS-PrePost4.3 eZSetup, improvements are made so adaptive mesh refinement along a curve can be made without the need to define any tools. In Figures 12-7, 12-8, 12-9, 12-10and 12-11, mesh pre-refinement along a curve is demonstrated on the fender outer case. The effect of different TCTOL values on the mesh refinement is obvious. The keyword *INCLUDE_TRIM is recommended to be used at all times to include the dynain file from a previous simulation, except in case where to-be-adapted sheet blank has no stress and strain information (no *INITIAL_STRESS_SHELL, and *INITIAL_- STRAIN_SHELL cards present in the sheet blank keyword or dynain file), then the keyword *INCLUDE must be used. Adaptive mesh refinement along a curve during trimming: When this keyword *ELEMENT_TRIM is present, this keyword is used to refine meshes during a trimming simulation. Coarse meshes along the trim curve can be refined prior to trimming, leaving a more detailed and distinctive trim edge. A partial example input deck is shown below: *INCLUDE_TRIM drawn.dynain *ELEMENT_TRIM 1 *DEFINE_CURVE_TRIM_NEW $# TCID TCTYPE TFLG TDIR TCTOL TOLN NSEED1 NSEED2 1 2 0 0.250 1 doubletrim.iges *DEFINE_TRIM_SEED_POINT_COORDINATES $ NSEED X1 Y1 Z1 X2 Y2 Z2 1 -184.565 84.755 *CONTROL_ADAPTIVE_CURVE $# IDSET ITYPE N SMIN ITRIOPT 1 2 3 3.0 0 *CONTROL_CHECK_SHELL $# PSID IFAUTO CONVEX ADPT ARATIO ANGLE SMIN 1 1 1 1 0.25 150.0 0.18 Where the keyword *ELEMENT_TRIM is used to define a deformable part set to be trimmed. The keyword *DEFINE_CURVE_TRIM_NEW is used to define the trim curve and keyword *DEFINE_TRIM_SEED_POINT_COORDINATES is used to define a seed point coordinate located on the portion that remains after trimming. The keyword tolerance, along type, with trim The etc. *CONTROL_ADAPTIVE_CURVE is used to define the adaptive mesh refinement level and minimum element size along the keyword the *CONTROL_CHECK_SHELL is used to repair and fix trimmed elements so they are suitable for next stage simulation. More details can be found in each of the corresponding keyword manual section. trim curve. Finally, Figure 12-4. Mesh refinement along a curve Curves defining adaptive mesh location Formed blank Figure 12-5. Curves can be discontinuous and in one IGES file. Figure 12-6. Define variable TCTOL to limit the mesh adaptivity area. TCTOL Trim panel Curve defining pre-adaptive area Flanging area mating with hood inner Figure 12-7. A complex mesh refinement example (NUMISHEET2002 Fender). Curve defining center of adaptive band Figure 12-8. Original mesh with target curves defined. Figure 12-9. Mesh refinement with TCTOL = 0.5. 0.5 mm 1.0 mm Figure 12-10. Mesh refinement with TCTOL = 1.0. 2.0 mm Figure 12-11. Mesh refinement with TCTOL = 2.0. *CONTROL_ALE Purpose: Set global control parameters for the Arbitrary Lagrangian-Eulerian (ALE) and Eulerian calculations. This command is required when solid element formulation 5, 6, 7, 11, or 12 is used. Parallel processing using SMP is not recommended when using these element formulations, rather it is better to use MPP for good parallel processing performance. See *CONTROL_MPP_DECOMPOSITION_DISTRIBUTE_ALE_ELE- MENTS. Card 1 1 2 3 4 5 6 7 8 Variable DCT NADV METH AFAC BFAC CFAC DFAC EFAC Type Default I 1 Card 2 1 I 0 2 I 1 3 F 0 4 F 0 5 F 0 6 F 0 7 F 0 8 Variable START END AAFAC VFACT PRIT EBC PREF NSIDEBC Type Default F 0 F 1020 F 1 F F 10-6 0.0 I 0 F I 0.0 none This card is optional. Card 3 1 2 3 4 5 6 7 8 Variable NCPL NBKT IMASCL CHECKR BEAMIN MMGPREF PDIFMX DTMUFAC Type Default I 1 I 50 I 0 F F 0.0 0.0 I 0 F F 0.0 0.0 *CONTROL Card 4 1 2 3 4 5 6 7 8 Variable OPTIMPP Type Default I 0 VARIABLE DCT DESCRIPTION Flag to invoke alternate advection logic. Formerly flag to control default continuum treatment: NE.-1: Use default advection logic. EQ.-1: Use alternate advection logic; generally recommended, especially for simulation of explosives . NADV Number of cycles between advections (almost always set to 1). METH Advection method: EQ.1: Donor cell with Half Index Shift (HIS), first order accurate. EQ.2: Van Leer with HIS, second order accurate. EQ.-2: Van Leer with HIS: Additionally,the monotonicity condition is relaxed during advection process to better preserve *MAT_HIGH_EXPLOSIVE_BURN material interfaces. EQ.3: Donor cell with HIS modified to conserve total energy over each advection step, in contrast to METH = 1 which conserving internal energy . AFAC ALE smoothing weight factor - Simple average: EQ.-1: turn smoothing off: . BFAC CFAC DFAC ALE smoothing weight factor – Volume weighting ALE smoothing weight factor – Isoparametric ALE smoothing weight factor – Equipotential VARIABLE DESCRIPTION EFAC ALE smoothing weight factor – Equilibrium START END Start time for ALE smoothing or start time for ALE advection if smoothing is not used. End time for ALE smoothing or end time for ALE advection if smoothing is not used. AAFAC ALE advection factor (donor cell options, default = 1.0) VFACT Volume fraction limit for stresses in single material and void formulation. All stresses are set to zero for elements with lower volume fraction than VFACT. EQ.0.0: set to default 10−6 PRIT A flag to turn on or off the pressure equilibrium iteration option for multi-material elements . EQ.0: Off (default) EQ.1: On EBC Automatic Eulerian boundary condition . EQ.0: Off EQ.1: On with stick condition EQ.2: On with slip condition PREF NSIDEBC NCPL Reference pressure to compute the internal forces. . A node set ID (NSID) which is to be excluded from the EBC constraint. Number of Lagrangian cycles between coupling calculations. This is typically done every cycle; therefore, its default is 1. This is on optional card 3. NBKT IMASCL *CONTROL DESCRIPTION Number of Lagrangian cycles between global bucket-sort searches to locate the position of the Lagrangian structure (mesh) relative to the ALE fluid (mesh). Default is 50. This is on optional card 3. LT.0: |NBKT| is a *DEFINE_CURVE ID defining a table: time vs NBKT as defined above EQ.0: (Default) NBKT = 50: If the mesh is moving, NBKT is adapted for the buckets to follow the mesh more closely GT.0: NBKT remains constant. A flag for turning ON/OFF mass scaling for ALE parts. The global mass scaling control (parameter DT2MS under *CON- TROL_TIMESTEP card) must be ON. If the run dt is lower than the mass scaling dt, then IMASCL has the following effects: EQ.0: (Default) No mass scaling for ALE parts. Print out maximum 20 warnings. EQ.1: No mass scaling for ALE parts. Stop the run. EQ.2: Do mass scaling for ALE parts (the result may not be correct due to this scaling). EQ.3: No mass scaling for ALE parts. Timestep is taken as the minimum of the ALE timestep and DT2MS. CHECKR BEAMIN A parameter for reducing or eliminating an ALE pressure locking pattern. It may range from 0.01 to 0.1 . Flag to align the dynamics of plain strain and axisymmetric beams in 2D FSI ALE models to their shell counterparts in 3D FSI ALE models: EQ.0.0: Off (default) EQ.1.0: On MMGPREF *CONTROL_ALE DESCRIPTION MMGPREF selects the method that is used to include a reference pressure in a calculation involving ALE multi-material groups . LT.0: |MMGPREF| is the id of a table defined by *DEFINE_- CURVE where the abscissas are the multi-material group ids and the ordinates are the reference pressures. If a multi-material group is not in the table, its reference pressure is default to PREF. For situations in which the reference pressures are time dependent *DEFINE_TABLE should be used instead of *DEFINE_CURVE. The table should consist of a set of curves indexed by group ID that encode reference pres- sure as a function of time. If 𝑛 groups need reference pressure histories, *DEFINE_TABLE will have 𝑛 lines followed by 𝑛 corresponding *DEFINE_CURVE. EQ.0: Off (default). EQ.1: Obsolete: Use MMGPREF < 0 instead EQ.2: Obsolete: Use MMGPREF < 0 instead PDIFMX Maximum of pressure difference between neighboring ALE elements under which the stresses are zeroed out: EQ.0: Off (default) GT.0: On DTMUFAC Scale a time step called DTMU that depends on the dynamic viscosity 𝜇, the initial density 𝜌, and an element characteristic length ℓ: DTMU = 𝜌ℓ2 2𝜇 DTMU is emitted by the element to the solver as an element time step, thereby making DTMU an upper bound on the global time step. EQ.0: Off (default) GT.0: On Optimize the MPP communications in the penalty coupling (*CONSTRAINED_LAGRANGE_IN_SOLID, CTYPE = 4) and group ALE parts together for the element processing. EQ.0: Off (default) EQ.1: On *CONTROL_ALE VARIABLE OPTIMPP Remarks: 1. The PRIT Field. Most of the fast transient applications do not need this feature. It could be used in specific slow dynamic problems for which material constitu- tive laws with very different compressibility are linear and the stresses in multi- material elements require to be balanced. 2. The EBC Field. This option, used for EULER formulations. It automatically defines velocity boundary condition constraints for the user. The constraints, once defined, are applied to all nodes on free surfaces of an Eulerian domain. For problems where the normal velocity of the material at the boundary is zero such as injection molding problems, the automatic boundary condition parame- ter is set to 2. This will play the same role as the nodal single point constraint. For EBC = 1, the material velocity of all free surface nodes of an Eulerian do- main is set to zero. 3. The PREF Field. The reference pressure PREF is subtracted from the stresses before computing the internal forces. Thus PREF is equivalent to applying a *LOAD_SEGMENT card to balance the internal pressure along the ALE mesh boundaries. PREF is applied to all the materials in the ALE mesh. So, before the subtraction for MMGPREF > 0, PREF is added to the stresses of some mate- rials. On another hand, MMGPREF < 0 subtracts a reference pressure depending on ALE MMG ID. The shift of the stresses by PREF is not necessary (and so it can not be seen in the LS-PrePost fringe of the pressures). For example, if a model has 3 ALE groups: air with an initial pressure of 1.0 bar, an explosive material, and water, the reference pressure of the first group would be 1.0 bar whereas the other groups would have none. In that case, PREF = 0.0 bar and MMGPREF = -LCID where LCID is the id of the following table: *DEFINE_CURVE lcid 1,1.0 2,0.0 3,0.0 4. CHECKR Field for One Point Integration. Due to one point integration, ALE elements may experience a spatial instability in the pressure field referred to as checker boarding. CHECKR is a scale for diffusive flux calculation to alleviate this problem. 5. METH=3 for Conserving Total Energy. Generally, it is not possible to conserve both momentum and kinetic energy (KE) at the same time. Typically, internal energy (IE) is conserved and KE may not be. This may result in some KE loss (hence, total energy loss). For many analyses this is tolerable, but for airbag application, this may lead to the reduction of the inflating potential of the inflator gas. METH=3 tries to eliminate this loss in KE over the advection step by storing any loss KE under IE, thus conserving total energy of the sys- tem. 6. Smoothing Factors. All the smoothing factors (AFAC, BFAC, CFAC, DFAC, EFAC) are generally most applicable to ELFORM = 5 (single material ALE for- mulation). The ALE smoothing feature is not supported by MPP versions. 7. First Pass Recommendations. Although this card has many parameters, only a few are required definitions. Typically, one can try setting NADV=1, METH=1, AFAC=-1 and the rest as “0” as a starting point. Sometimes when needed, PREF should be defined. This is adequate for most cases. Sometimes it may be appropriate to fine-tune the model by changing METH to 2 or 3 de- pending on the physics. 8. Pressure Checker Boarding. Because the internal forces are located at the nodes, while the pressure is stored at the element center, sometimes a "checker- board pattern" arises in the pressure distribution. It is a kind of locking effect that normally occurs only in problems having very small volumetric strains, i.e., at small pressures. “CHECKR” is designed for alleviating this problem. 9. The DCT Field. Starting with the R5 the DCT field can be used to invoke an alternate advection scheme. DCT=-1 is recommended over the default scheme, especially for simulating explosives and includes the following major changes: a) Relaxes an artificial limit on the expansion ratio limit. The default limit improves stability in some situations but can overestimate the explosive impulse. b) Corrects redundant out-flux of material at corner elements. The redun- dancy can lead to negative volume. c) Removes several artificial constraints in the advection which were origi- nally implemented to assist in stability but are no longer needed. 10. METH = -2. The METH = -2 advection type is the same as METH = 2 with only one exception. It employs a looser constraint on monotonicity requirement during ALE advection. When METH = 2, for each advection process along three directions (front/back, top/bottom, left/right), the maximum/minimum values for advected history variables in the three elements along that direction are capped. METH = -2 relaxed the monotonicity condition so that the advec- ted value is capped at the maximum/minimum value in the element itself and its neighboring 26 elements. This option, in certain conditions, can better pre- serve the material interface for materials defined with *MAT_HIGH_EXPLO- SIVE_BURN. *CONTROL_BULK_VISCOSITY Purpose: Reset the default values of the bulk viscosity coefficients globally. This may be advisable for shock wave propagation and some materials. Bulk viscosity is used to treat shock waves. A viscous term q is added to the pressure to smear the shock discontinuities into rapidly varying but continuous transition regions. With this method the solution is unperturbed away from a shock, the Hugoniot jump conditions remain valid across the shock transition, and shocks are treated automatically. Card 1 Variable 1 Q1 Type F 2 Q2 F Default 1.5 .06 3 4 5 6 7 8 TYPE BTYPE I 1 I 0 VARIABLE DESCRIPTION Q1 Q2 Default quadratic viscosity coefficient. Default linear viscosity coefficient. TYPE Default bulk viscosity type, IBQ (Default = 1) EQ.-2: standard (also types 2, 4, 10, 16, and 17). With this option the internal energy dissipated by the viscosity in the shell elements is computed and included in the overall energy balance. EQ.-1: standard (also types 2, 4, 10, 16, and 17 shell elements). The internal energy is not computed in the shell ele- ments. EQ.+1: standard: Solid elements only and internal energy is always computed and included in the overall energy balance. EQ.+2: Richards-Wilkins: Two-dimensional plane strain and axisymmetric solid elements only. Internal energy is always computed and included in the overall energy balance. VARIABLE DESCRIPTION BTYPE Beam bulk viscosity type (Default = 0) EQ.0: The bulk viscosity is turned off for beams. EQ.1: The bulk viscosity is turned on for beam types 1 and 11. The energy contribution is not included in the overall energy balance. EQ.2: The bulk viscosity is turned on for beam type 1 and 11. The energy contribution is included in the overall energy balance. Remarks: The bulk viscosity creates an additional additive pressure term given by: 𝑞 = { 𝜌𝑙(𝑄1𝑙𝜀̇𝑘𝑘 2 − 𝑄2𝑎𝜀̇𝑘𝑘) 𝜀̇𝑘𝑘 < 0 𝜀̇𝑘𝑘 ≥ 0 where 𝑄1 and 𝑄2 are dimensionless input constants which default to 1.5 and .06, respectively, and 𝑙 is a characteristic length given as the square root of the area in two dimensions and as the cube root of the volume in three, 𝑎 is the local sound speed, 𝑄1 defaults to 1.5 and 𝑄2 defaults to .06. See Chapter 21 in the LS-DYNA Theory Manual for more details. The Richards-Wilkins, see [Richards 1965, Wilkins 1976], bulk viscosity considers the directional properties of the shock wave. This has the effect of turning off the bulk viscosity in converging geometries minimizing the effects of “q-heating”. The standard option is active whenever the volumetric strain rate is undergoing compression even though no shock waves are present. Purpose: Check for various problems in the mesh. *CONTROL_CHECK_SHELL Part cards. Include one card for each part or part set to be checked. The next keyword (“*”) card terminates this input. Card 1 1 2 3 4 5 6 7 8 Variable PSID IFAUTO CONVEX ADPT ARATIO ANGLE SMIN Type Default I 0 I 0 I 1 I 1 F F F 0.25 150.0 0.0 VARIABLE DESCRIPTION PSID Part or part set ID to be checked: EQ.0: do not check GT.0: part ID LT.0: part set ID IFAUTO Flag to automatically correct bad elements: EQ.0: write warning message only EQ.1: fix bad element, write message CONVEX Check element convexity (internal angles less than 180 degrees) EQ.0: do not check EQ.1: check ADPT Check adaptive constraints EQ.0: do not check EQ.1: check ARATIO Minimum allowable aspect ratio. Elements which do not meet minimum aspect ratio test will be treated according to IFAUTO above. ANGLE Maximum allowable internal angle. Elements which fail this test will be treated according to IFAUTO above. DESCRIPTION Minimum element size. Elements which fail this test will be treated according to IFAUTO above. VARIABLE SMIN Remarks: 1. For the SHELL option, shell element integrity checks which have been identified as important in metal forming applications are performed. These checks can improve springback convergence and accuracy. This option will repair bad elements created, for example, during trimming operations. 2. 3. If the convexity test is activated, all failed elements will be fixed regardless of IFAUTO. In addition to illegal constraint definitions (slave which is also a master), checks are performed for mesh connectivities which have been found to cause conver- gence trouble in implicit springback applications. 4. Variable SMIN should be set to 1/4 to 1/3 of smallest pre-trim element length. In an example below, smallest element length pre-trim is 0.6mm, which makes SMIN to be 0.18: *CONTROL_CHECK_SHELL 1,1,1,1,0.25,150.0,0.18 $ smin=(0.25~0.3)*smallest pre-trim element length, which is ~0.6 mm. 5. Shell checking is done during the input phase (in sprinback input deck) in LS- DYNA R5 Revision 63063 and prior releases. After the Revision, it is done after trimming is completed. Therefore the keyword should be included in a trim- ming input deck. *CONTROL_COARSEN Purpose: Adaptively de-refine (coarsen) a shell mesh by selectively merging four adjacent elements into one. Adaptive constraints are added and removed as necessary. Card 1 1 2 3 4 5 6 7 8 Variable ICOARSE ANGLE NSEED PSID SMAX Type Default Card 2 Variable Type Default I 0 1 N1 I 0 F none 2 N2 I 0 I 0 3 N3 I 0 I 0 4 N4 I 0 F 0 5 N5 I 0 VARIABLE DESCRIPTION ICOARSE Coarsening flag: EQ.0: do not coarsen (default) 6 N6 I 0 7 N7 I 0 8 N8 I 0 EQ.1: coarsen mesh at beginning of simulation for forming model EQ.2: coarsen mesh at beginning of simulation for crash model ANGLE Allowable angle change between neighboring elements. Adjacent elements which are flat to within ANGLE degrees are merged. (Suggested starting value = 8.0 degrees) NSEED Number of seed nodes (optional). EQ.0: use only automatic searching. GT.0: the number of seed nodes with which to supplement the search algorithm. See Remark 2. NSEED must be an integer less than or equal to 8. VARIABLE DESCRIPTION PSID SMAX Part set ID. All the parts defined in this set will be prevented from been coarsened. Maximum element size. For ICOARSE = 2, no elements larger than this size will be created. N1, …, N8 Optional list of seed node IDs for extra searching. If no seed nodes are specified, leave card 2 blank. Remarks: 1. Coarsening is performed at the start of a simulation. The first plot state represents the coarsened mesh. By setting the termination time to zero and including the keyword *INTERFACE_SPRINGBACK_LSDYNA a keyword input deck can be generated containing the coarsened mesh. 2. By default, an automatic search is performed to identify elements for coarsen- ing. In some meshes, isolated regions of refinement may be overlooked. Seed nodes can be identified in these regions to assist the automatic search. Seed nodes identify the central node of a four-element group which is coarsened into a single element if the angle criterion is satisfied. 3. The keyword *DEFINE_BOX_COARSEN can be used to indicate regions of the mesh which are protected from coarsening. *CONTROL_CONTACT Purpose: Change defaults for computation with contact surfaces. Card 1 1 2 3 4 5 6 7 8 Variable SLSFAC RWPNAL ISLCHK SHLTHK PENOPT THKCHG ORIEN ENMASS Type F F Default .1 none Remarks Card 2 1 2 I 1 3 3 I 0 I 1 I 0 I 1 I 0 4 5 6 7 8 Variable USRSTR USRFRC NSBCS INTERM XPENE SSTHK ECDT TIEDPRJ Type Default I 0 I 0 I 10-100 I 0 F 4.0 I 0 I 0 I 0 Remaining cards are optional.† The optional cards apply only to the following contact types: *SINGLE_SURFACE *AUTOMATIC_GENERAL *AUTOMATIC_SINGLE_SURFACE *AUTOMATIC_NODES_TO_… *AUTOMATIC_SURFACE_… *AUTOMATIC_ONE_WAY_… *ERODING_SINGLE_SURFACE. The friction coefficients SFRIC, DFRIC, EDC, and VFC are active only when *PART_- CONTACT is invoked with FS = -1 in *CONTACT, and the corresponding frictional coefficients in *PART_CONTACT are set to zero. This keyword’s TH, TH_SF, and PEN_SF override the corresponding parameters in *CONTACT, but will not override corresponding nonzero parameters in *PART_CONTACT. Card 3 1 2 3 4 Variable SFRIC DFRIC EDC VFC Type F F F F 5 TH F 6 7 8 TH_SF PEN_SF PTSCL F F F Default 0.0 0.0 0.0 0.0 0.0 0.0 0.0 1.0 Card 4 1 2 3 4 5 6 7 8 Variable IGNORE FRCENG SKIPRWG OUTSEG SPOTSTP SPOTDEL SPOTHIN Type Default I 0 Card 5 1 I 0 2 I 0 3 I 0 4 I 0 5 I F 0 inactive 6 7 8 Variable ISYM NSEROD RWGAPS RWGDTH RWKSF ICOV SWRADF ITHOFF Type Default I 0 I 0 I 0 F 0. F 1.0 I 0 F 0. I Card 6 1 2 3 4 5 6 7 8 Variable SHLEDG PSTIFF ITHCNT TDCNOF FTALL SHLTRW IGACTC Type Default I 0 I 0 I 0 I 0 I 0 F 0. I 0 VARIABLE DESCRIPTION SLSFAC Scale factor for sliding interface penalties, SLSFAC: EQ.0: default = .1. RWPNAL Scale factor for rigid wall penalties, which treat nodal points interacting with rigid walls, RWPNAL. The penalties are set so that an absolute value of unity should be optimal; however, this penalty value may be very problem dependent. If rig- id/deformable materials switching is used, this option should be used if the switched materials are interacting with rigid walls. LT.0.0: all nodes are treated by the penalty method. This is required for implicit calculations. Since seven (7) vari- ables are stored for each slave node, only the nodes that may interact with the wall should be included in the node list. EQ.0.0: the constraint method is used and nodal points which belong to rigid bodies are not considered. GT.0.0: rigid bodies nodes are treated by the penalty method and all other nodes are treated by the constraint meth- od. ISLCHK Initial penetration check in contact surfaces with indication of initial penetration in output files : EQ.0: the default is set to 1, EQ.1: no checking, EQ.2: full check of initial penetration is performed. VARIABLE SHLTHK DESCRIPTION Flag for consideration of shell thickness offsets in non-automatic surface-to-surface and non-automatic nodes-to-surface type contacts. Shell thickness offsets are always included in single surface, constraint-based, automatic surface-to-surface, and automatic nodes-to-surface contact types : EQ.0: thickness is not considered, EQ.1: thickness is considered but rigid bodies are excluded, EQ.2: thickness is considered including rigid bodies. PENOPT Penalty stiffness value option. For default calculation of the penalty value please refer to the LS-DYNA Theory Manual. EQ.0: the default is set to 1, EQ.1: minimum of master segment and slave node (default for most contact types), EQ.2: use master segment stiffness (old way), EQ.3: use slave node value, EQ.4: use slave node value, area or mass weighted, EQ.5: same as 4 but inversely proportional to the shell thickness. This may require special scaling and is not generally recommended. Options 4 and 5 can be used for metal forming calculations. THKCHG Shell thickness changes considered in single surface contact: EQ.0: no consideration (default), EQ.1: shell thickness changes are included. ORIEN Optional automatic reorientation of contact interface segments during initialization. See Remark 4. EQ.0: default is set to 1. EQ.1: active for automated (part) input only. Contact surfaces are given by *PART definitions. EQ.2: active for manual (segment) and automated (part) input. EQ.3: inactive for non-forming contact. EQ.4: inactive for *CONTACT_FORMING types and *CON- TACT_DRAWBEAD. ENMASS USRSTR USRFRC NSBCS *CONTROL_CONTACT DESCRIPTION Treatment of the mass of eroded nodes in contact. This option affects all contact types where nodes are removed after surrounding elements fail. Generally, the removal of eroded nodes makes the calculation more stable; however, in problems where erosion is important the reduction of mass will lead to incorrect results. ENMASS is not supported when SOFT = 2 on optional card A. EQ.0: eroding nodes are removed from the calculation. EQ.1: eroding nodes of solid elements are retained and continue to be active in contact. EQ.2: the eroding nodes of solid and shell elements are retained and continue to be active in contact. Storage per contact interface for user supplied interface control subroutine, see Appendix F. If zero, no input data is read and no interface storage is permitted in the user subroutine. This storage should be large enough to accommodate input parameters and any history data. This input data is available in the user supplied subroutine. Storage per contact interface for user supplied interface friction subroutine, see Appendix G. If zero, no input data is read and no interface storage is permitted in the user subroutine. This storage should be large enough to accommodate input parameters and any history data. This input data is available in the user supplied subroutine. Number of cycles between contact searching using three dimensional bucket searches, defaults recommended. For Mortar contact (option MORTAR on the CONTACT card), the default is 100. INTERM Flag for intermittent searching in old surface-to-surface contact using the interval specified as NSBCS above: EQ.0: off, EQ.1: on. VARIABLE XPENE DESCRIPTION Contact surface maximum penetration check multiplier. If the small penetration checking option, PENCHK, on the contact surface control card is active, then nodes whose penetration then exceeds the product of XPENE and the element thickness are set free, see *CONTACT_OPTION_… EQ.0: default is set to 4.0. SSTHK Flag for using actual shell thickness in single surface contact logic-types 4, 13, 15 and 26. See Remarks 1 and 2. EQ.0: Actual shell thickness is not used in the contacts. (default), EQ.1: Actual shell thickness is used in the contacts. (sometimes recommended for metal forming calculations). ECDT Time step size override for eroding contact: EQ.0: contact time size may control Dt. EQ.1: contact is not considered in Dt determination. TIEDPRJ Bypass projection of slave nodes to master surface in types: *CONTACT_TIED_NODES_TO_SURFACE *CONTACT_TIED_SHELL_EDGE_TO_SURFACE *CONTACT_TIED_SURFACE_TO_SURFACE Tied interface options: EQ.0: eliminate gaps by projection nodes, EQ.1: bypass projection: Gaps create rotational constraints which can substantially affect results. SFRIC Default static coefficient of friction DFRIC Default dynamic coefficient of friction EDC VFC TH Default exponential decay coefficient Default viscous friction coefficient Default contact thickness TH_SF Default thickness scale factor VARIABLE DESCRIPTION PEN_SF Default local penalty scale factor PTSCL IGNORE Scale factor on the contact stress exerted onto shells formulations 25, 26, and 27. When DOF = 3 the scale factor also applies to shell formulations 2, and 16. Ignore initial penetrations in the *CONTACT_AUTOMATIC options. In the SMP contact this flag is not implement for the AU- TOMATIC_GENERAL option. “Initial” in this context refers to the first timestep that a penetration is encountered. This option can also be specified for each interface on the third optional card under the keyword, *CONTACT. The value defined here will be the default. EQ.0: move nodes to eliminate initial penetrations in the model definition. EQ.1: allow initial penetrations to exist by tracking the initial penetrations. EQ.2: allow initial penetrations to exist by tracking the initial penetrations. However, penetration warning messages are printed with the original coordinates and the recom- mended coordinates of each slave node given. FRCENG Flag to activate the calculation of frictional sliding energy: EQ.0: do not calculate, EQ.1: calculate frictional energy in contact and store as “Surface Energy Density” in the binary INTFOR file. Convert mechanical frictional energy to heat when doing a coupled thermal-mechanical problem. When PKP_- SEN = 1 on the keyword card *DATABASE_EXTENT_BI- NARY, it is possible to identify the energies generated on the upper and lower shell surfaces, which is important in metal forming applications. This data is mapped after each H-adaptive remeshing. EQ.2: Same as behavior as above (set to 1) except that frictional energy is not converted to heat. VARIABLE DESCRIPTION SKIPRWG Flag not to display stationary rigid wall by default. EQ.0: generate 4 extra nodes and 1 shell element to visualize stationary planar rigid wall. EQ.1: do not generate stationary rigid wall. OUTSEG Flag to output each beam spot weld slave node and its master segment for contact type: *CONTACT_SPOTWELD into the d3hsp file. EQ.0: no, do not write out this information. EQ.1: yes, write out this information. SPOTSTP If a spot weld node or face, which is related to a *MAT_- SPOTWELD beam or solid element, respectively, cannot be found on the master surface, should an error termination occur? SPOTDEL EQ.0: no, silently delete the weld and continue, EQ.1: yes, print error message and terminate, EQ.2: no, delete the weld, print a message, and continue, EQ.3: no, keep the weld. This is not recommended as it can lead to instabilities. This option controls the behavior of spotwelds when the parent element erodes. When SPOTDEL is set to 1, the beam or solid spotweld is deleted and the tied constraint is removed when the parent element erodes. Parent element is the element to which the slave node is attached using the TIED interface. This option also works for SPRs, i.e. they automatically fail if at least one of the parent elements fails. To avoid instabilities, this option is recommended to be set to 1 for any situation in which the parent element is expected to erode. EQ.0: no, do not delete the spot weld beam or solid element or SPR, EQ.1: yes, delete the weld elements or SPRs when the attached shells on one side of the element fail. On vector processors this option can significantly slow down the calculation if many weld elements fail since the vector lengths are reduced. On non-vector processors the cost-penalty is minimal. SPOTHIN *CONTROL_CONTACT DESCRIPTION Optional thickness scale factor. If active, define a factor greater than zero, but less than one. Premature failure of spot welds can occur due to contact of the spot welded parts in the vicinity of the spot weld. This contact creates tensile forces in the spot weld. Although this may seems physical, the compressive forces generated in the contact are large enough to fail the weld in tension before failure is observed in experimental test. With this option, the thickness of the parts in the vicinity of the weld are automatically scaled, the contact forces do not develop, and the problem is avoided. We recommend setting the IGNORE option to 1 or 2 if SPOTHIN is active. This option applies only to the AUTOMATIC_SINGLE_SURFACE option. See Remark 5. ISYM Symmetry plane option default for automatic segment generation when contact is defined by part ID’s: EQ.0: off, EQ.1: do not include faces with normal boundary constraints (e.g., segments of brick elements on a symmetry plane). This option is important to retain the correct boundary conditions in the model with symmetry. NSEROD Flag to use one-way node to surface erosion EQ.0: use two-way algorithm EQ.1: use one-way algorithm RWGAPS Flag to add rigid wall gap stiffness, see parameter RWGDTH below. EQ.1: add gap stiffness EQ.2: do not add gap stiffness RWGDTH RWKSF Death time for gap stiffness. After this time the gap stiffness is no longer added. Rigid wall penalty scale factor for contact with deformable parts during implicit calculations. This value is independent of SLS- FAC and RWPNAL. If RWKSF is also specified in *RIGID- WALL_PLANAR, the stiffness is scaled by the product of the two values. VARIABLE ICOV DESCRIPTION the covariant Invokes formulation of Konyukhov and Schweizerhof in the FORMING contact option. This option is available in the third revision of version 971, but is not recommended since it is still being implemented. EQ.0: standard formulation (default) EQ.1: covariant contact formulation. SWRADF Spot weld radius scale factor for neighbor segment thinning EQ.0: neighbor segments not thinned (default) GT.0: The radius of beam spot welds are scaled by SWRADF when searching for close neighbor segments to thin. ITHOFF Flag for offsetting thermal contact surfaces for thick thermal shells EQ.0: No offset, if thickness is not included in the contact the heat will be transferred between the mid-surfaces of the corresponding contact segments (shells). EQ.1: Offsets are applied so that contact heat transfer is always between the outer surfaces of the contact segments (shells). SHLEDG Flag for assuming edge shape for shells when measuring penetration. This is available for segment based contact EQ.0: Shell edges are assumed round (default), EQ.1: Shell edges are assumed square and are flush with the nodes PSTIFF Flag to choose the method for calculating the penalty stiffness. This is available for segment based contact . See Remark 6. EQ.0: Based on material density and segment dimensions (default), EQ.1: Based on nodal masses. VARIABLE DESCRIPTION ITHCNT Thermal contact heat transfer methodology LT.0: conduction evevenly distributed (pre R4) EQ.0: default set to 1 EQ.1: conduction weighted by shape functions, reduced intergration EQ.2: conduction weighted by shape functions, full integration TDCNOF Tied constraint offset contact update option. EQ.0: Update velocities and displacements from accelerations EQ.1: Update velocities and accelerations from displacements. This option is recommended only when there are large angle changes where the default does not maintain a constant offset to a small tolerance. This latter option is not as stable as the default and may require additional damping for stability. See *CONTROL_BULK_VISCOSI- TY and *DAMPING_PART_STIFFNESS. Option to output contact forces to RCFORC for all 2 surface force transducers when the force transducer surfaces overlap. See Remark 7. EQ.0: Output to the first force transducer that matches (default) EQ.1: Output to all force transducers that match. FTALL SHLTRW Optional shell thickness scale factor for contact with rigid walls. Shell thickness is not considered when SHLTRW = 0 (default). SHLTRW = 0.5 will result in an offset of half of shell thickness in contact with rigid walls. IGACTC Options to use isogeometric shells for contact detection when contact involves isogeometric shells: EQ.0: contact between interpolated nodes and interpolated shells EQ.1: contact between interpolated nodes and isogeometric shells *CONTROL 1. Shell Thickness. The shell thickness change option (ISTUPD) must be activated in *CONTROL_SHELL and a nonzero flag specified for SHLTHK above before the shell thickness changes can be included in the surface-to- surface contact types. If thickness changes are to be included in the single sur- face contact algorithms, an additional flag must be set, see THKCHG above. Although the contact algorithms that include the shell thickness are relatively recent, they work in parallel (MPI) Dyna are fully optimized. The searching in these algorithms is considerably more extensive and therefore slightly more expensive. 2. Upper Limit on Thickness. In the single surface contacts types SINGLE_SUR- FACE, AUTOMATIC_SINGLE_SURFACE, AUTOMATIC_GENERAL, AU- TOMATIC_GENERAL_INTERIOR and ERODING_SINGLE_SURFACE, the default contact thickness is taken as the smaller of two values — the shell thick- ness or 40% of the minimum edge length. (NOTE: Minimum edge length is calculated as min(N4-to-N1, N1-to-N2, N2-to-N3). N3-to-N4 is neglected ow- ing to the possibility of the shell being triangular.) This may lead to unexpected results if it is the intent to include thickness effects when the in-plane shell element dimensions are less than the thickness. The default is based on years of experience where it has been observed that sometimes rather large nonphysical thicknesses are specified to achieve high stiffness values. Since the global searching algorithm includes the effects of shell thicknesses, nonphysical thick- ness dimensions slow the search down considerably. 3. Initial Penetration Check. As of version 950 the initial penetration check option is always performed regardless of the value of ISLCHK. If you do not want to remove initial penetrations then set the contact birth time so that the contact is not active at time 0. 4. Automatic Reorientation. Automatic reorientation requires offsets between the master and slave surface segments. The reorientation is based on segment connectivity and, once all segments are oriented consistently based on connec- tivity, a check is made to see if the master and slave surfaces face each other based on the right hand rule. If not, all segments in a given surface are reori- ented. This procedure works well for non-disjoint surfaces. If the surfaces are disjoint, the AUTOMATIC contact options, which do not require orientation, are recommended. In the FORMING contact options automatic reorientation works for disjoint surfaces. 5. Neighbor Segment Thinning Option. If SPOTHIN is greater than zero and SWRADF is greater than zero, a neighbor segment thinning option is active. The radius of a beam spot weld is scaled by SWRADF, and then a search is made for shell segments that are neighbors of the tied shell segments that are touched by the weld but not tied by it. 6. Segment Masses for Penalty Stiffness. Segment based contact calculates a penalty stiffness based on the solution time step and the masses of the segments in contact. By default, segment masses are calculated using the material density of the element associated with the seg- ment and the volume of the segment. This method does not take into account added mass introduced by lumped masses or mass scaling and can lead to stiffness that is too low. Therefore, a second method (PSTIFF = 1) was added which estimates the segment mass using the nodal masses. Setting a PSTIFF values here will set the default values for all interfaces. The PSTIFF option can also be specified for individual contact interfaces by defining PSTIFF on option- al card F of *CONTACT. 7. Force Transducer Search Option. Two surface force transducers measure the contact force from any contact interfaces that generate force between the slave and master surfaces of the force transducer. When contact is detected, a search is made to see if the contact force should be added to any 2 surface force trans- ducers. By default, when a force transducer match is found, the force is added and the search terminates. When FTALL = 1, the search continues to check for other two surface force transducer matches. This option is useful when the slave and master force transducer surfaces overlap. If there is no overlap, the default is recommended. *CONTROL Purpose: Change defaults for MADYMO3D/CAL3D coupling, see Appendix I. Card 1 1 2 3 4 5 6 7 8 Variable UNLENG UNTIME UNFORC TIMIDL FLIPX FLIPY FLIPZ SUBCYL Type F Default 1. F 1. F 1. F 0. I 0 I 0 I 0 I 1 VARIABLE UNLENG UNTIME UNFORC TIMIDL FLIPX DESCRIPTION Unit conversion factor for length. MADYMO3D/GM-CAL3D lengths are multiplied by UNLENG to obtain LS-DYNA lengths. Unit conversion factor for time, UNTIME. MADYMO3D/GM- CAL3D time is multiplied by UTIME to obtain LS-DYNA time. Unit conversion factor for force, UNFORC. MADYMO3D/GM- CAL3D force is multiplied by UNFORC to obtain LS-DYNA force. Idle time during which CAL3D or MADYMO is computing and LS-DYNA remains inactive. Important for saving computer time. Flag for flipping X-coordinate of CAL3D/MADYMO3D relative to the LS-DYNA model: EQ.0: off, EQ.1: on. FLIPY Flag for flipping Y-coordinate of CAL3D/MADYMO3D relative to the LS-DYNA model: EQ.0: off, EQ.1: on. FLIPZ Flag for flipping Z-coordinate of CAL3D/MADYMO3D relative to the LS-DYNA model: EQ.0: off, EQ.1: on. VARIABLE DESCRIPTION SUBCYL CAL3D/MADYMO3D subcycling interval (# of cycles): EQ.0: Set to 1, GT.0: SUBCYL must be an integer equal to the number of LS- DYNA time steps between each CAL3D/MADYMO3D step. Then the position of the contacting rigid bodies is assumed to be constant for n LS-DYNA time steps. This may result in some increase in the spikes in contact, thus this option should be used carefully. the CAL3D/MADYMO3D programs usually work with a very small number of degrees of freedom, not much gain in efficiency can be achieved. As *CONTROL Purpose: Global control parameters for CPM (Corpuscular Particle Method). Card 1 1 2 3 4 5 6 7 8 Variable CPMOUT NP2P NCPMTS CPMERR SFFDC Type I Default 11 I 5 I 0 I 0 F 1.0 VARIABLE DESCRIPTION CPMOUT Control CPM output database to the d3plot files: EQ.11: full CPM database in version 3 format (default) EQ.21: full CPM database in version 4 format EQ.22: CPM coordinates only in version 4 format EQ.23: CPM summary only in version 4 format NP2P Number of cycles for repartition particle among processors. This option is only used in LS-DYNA/MPP. (Default = 5) NCPMTS Time step size estimation: EQ.0: not consider CPM (default) EQ.1: use 1 micro-second as CPM time step size. This provides a better time step size if the model is made by rigid body. CPMERR EQ.0: disable checking and only output warning messages (Default) EQ.1: enable error checking. If LS-DYNA detects any problem, it will either error terminate the job or try to fix the prob- lem. Activated checks include: 1. Airbag integrity 2. Chamber integrity: this step applies the airbag integrity check to the chamber. 3. Inconsistent orientation between the shell refer- VARIABLE DESCRIPTION SFFDC Scale factor for the force decay constant. The default value is 1 and allowable arrange is [0.01,100]. ence geometry and FEM shell connectivity. Remarks: 1. D3PLOT Version. “Version 3” is an older format than “Version 4”. Version 4 stores data more efficiently than version 3 and has options for what data is stored, but may not be readable by old LS-PrePost executables. 2. Airbag Integrity Checking. The bag’s volume is used to evaluate all bag state variables. If the volume is ill-defined or inaccurate, then the calculation will fail. Therefore, it is vital that that the volume be closed, and that all shell nor- mal vectors point in the same direction. When CPMERR = 1 the calculation will error terminate if either the bag’s vol- ume is not closed or if one of its parts is not internally oriented (meaning that it contains elements that are not consistently oriented). Once it is verified that each part has a well-defined orientation, an additional check is performed to verify that all of bag’s constituent parts are consistently oriented with respect to each other. If they are not, then the part orientations are flipped until the bag is consistently oriented with an inward pointing normal vector. 3. Force Decay Constant. Particle impact force is gradually applied to airbag segment by a special smoothing function with the following form. 𝐹apply = [1 − exp ( −𝑑𝑡 SFFDC× 𝜏 )] (𝐹current + 𝐹stored) Where τ is the force decay constant stored in LS-DYNA. Purpose: Control CPU time. *CONTROL Card 1 1 2 3 4 5 6 7 8 Variable CPUTIM IGLST Type F I VARIABLE DESCRIPTION CPUTIM Seconds of CPU time: EQ.0.0: no CPU time limit set GT.0.0: time limit for cumulative CPU of the entire simulation, including all restarts. LT.0.0: absolute value is the CPU time limit in seconds for the first run and for each subsequent restart. IGLST Flag for outputting CPU and elapsed times in the “glstat” file EQ.0: no EQ.1: yes Remarks: The CPU limit is not checked until after the initialization stage of the calculation. Upon reaching the CPU limit, the code will output a restart dump file and terminate. The CPU limit can also be specified on the LS-DYNA execution line via “c=”. If a value is specified on both the execution line and in the input deck, the minimum value will be used. *CONTROL_DEBUG Purpose: Write supplemental information to the messag file(s). One effect of this command is that the sequence of subroutines called during initialization and memory allocation is printed. Aside from that, the extra information printed pertains only to a select few features, including: 1. Spot weld connections which use *MAT_100_DA and *DEFINE_CONNEC- TION_PROPERTIES. 2. The GISSMO damage model invoked using *MAT_ADD_EROSION. (Supple- mental information about failed elements is written.) *CONTROL_DISCRETE_ELEMENT Purpose: Define global control parameters for discrete element spheres. Card 1 1 2 3 4 5 6 7 8 Variable NDAMP TDAMP FRICS FRICR NORMK SHEARK CAP VTK Type Default F 0 F 0 F 0 F 0 F F 0.01 2/7 I 0 I 0 Capillary Card. Additional card for CAP ≠ 0. Card 2 1 2 3 4 5 6 7 8 Variable GAMMA VOL ANG GAP NBUF PARALLEL Type Default F 0 F 0 F 0 F 0 I 6 I 0 Card 3 is optional. If optional Card 3 is used, then Optional Card 2 must be defined. Card 3 1 2 3 4 5 6 7 8 Variable LNORM LSHEAR FRICD DC Type Default I 0 I 0 F FRICS F 0 VARIABLE DESCRIPTION NDAMP Normal damping coefficient TDAMP Tangential damping coefficient r1 r2 X1 X2 Figure 12-12. Schematic representation of sphere-sphere interaction VARIABLE DESCRIPTION FRICS Static coefficient of friction EQ.0: 3 DOF NE.0: 6 DOF (consider rotational DOF) FRICR Rolling friction coefficient NORMK Optional: scale factor of normal spring constant. Norm contact stiffness is calculated as 𝐾𝑛 = (Default = 0.01) {⎧ 𝑘1𝑟1𝑘2𝑟2 𝑘1𝑟1+𝑘2𝑟2 ⎩{⎨ |𝑁𝑂𝑅𝑀𝐾| 𝑖𝑓 𝑁𝑂𝑅𝑀𝐾 < 0 𝑁𝑂𝑅𝑀𝐾 𝑖𝑓 𝑁𝑂𝑅𝑀𝐾 > 0 SHEARK Optional: ratio between SHEARK/NORMK (Default = 2/7). Tangential stiffness is calculated as 𝐾𝑡 = 𝑆𝐻𝐸𝐴𝑅𝐾 ∙ 𝐾𝑛 CAP EQ.0: dry particles NE.0: wet particles, consider capillary additional input card. See Remark 1. force and need VTK Output DES in VTK format for ParaView EQ.0: no EQ.1: yes GAMMA Liquid surface tension, 𝛾 VOL Volume fraction VARIABLE DESCRIPTION ANG GAP Contact angle, 𝜃 Optional parameter affecting the spatial limit of the liquid bridge. CAP.EQ.0: GAP is ignored, if the CAP field is 0 and the simulation is modeling dry particles. CAP.NE.0: A liquid bridge exists when 𝛿, as illustrated in Figure 12-13, is less or equal to min(GAP, 𝑑rup) where 𝑑rup is the rupture distance of the bridge au- tomatically calculated by LS-DYNA . NBUF GE.0: Factor of memory use for asynchronous message buffer (Default = 6) LT.0: Disable asynchronous scheme and use minimum memory for data transfer PARALLEL EQ.0: skip contact force calculation for bonded DES (Default) EQ.1: consider contact force calculation for bonded DES LNORM LSHEAR FRICD Load curve ID of a curve that defines function for normal stiffness with respect to norm penetration ratio. See Remark 2. Load curve ID of a curve that defines function for shear stiffness with respect to norm penetration ratio. See Remark 3. Dynamic coefficient of friction. By default, FRICD = FRICS. The frictional coefficient is assumed to be dependent on the relative velocity 𝑣𝑟𝑒𝑙of the two DEM in contact 𝜇𝑐 = 𝐹𝑅𝐼𝐶𝐷 + (𝐹𝑅𝐼𝐶𝑆 − 𝐹𝑅𝐼𝐶𝐷)𝑒−𝐷𝐶∙∣𝑣𝑟𝑒𝑙∣. DC Exponential decay coefficient. The frictional coefficient is assumed to be dependent on the relative velocity 𝑣𝑟𝑒𝑙of the two DEM in contact 𝜇𝑐 = 𝐹𝑅𝐼𝐶𝐷 + (𝐹𝑅𝐼𝐶𝑆 − 𝐹𝑅𝐼𝐶𝐷)𝑒−𝐷𝐶∙∣𝑣𝑟𝑒𝑙∣. r1 r2 Figure 12-13. Schematic representation of capillary force model. Background: This method models all parts as being comprised of rigid spheres. These sphere interact with both conventional solids and other spheres. Sphere-sphere interactions are modeled in contact points using springs and dampers as illustrated in Figure 12-12. [Cundall & Strack 1979] Remarks: 1. Capillary Forces to Model Cohesion. This extension is enabled using the CAP field. Capillary force between wet particles is based on the following reference. “Capillary Forces between Two Spheres with a Fixed Volume Liquid Bridges: Theory and Experiment”, Yakov I. Rabinovich et al. Langmuir 2005, 21, 10992-10997. See Figure 12-13. The capillary force is given by where, and, 𝐹 = − 2𝜋𝑅𝛾𝑐𝑜𝑠𝜃 1 + 𝛿 2𝑑 , 𝑑 = ⎜⎛−1 + √1 + 2 ⎝ 2𝑉 𝜋𝑅𝛿2 ⎟⎞, ⎠ 𝑅 = 2𝑟1𝑟2 𝑟1 + 𝑟2 . 2. For two interacting DEMs with user defined curve for norm stiffness y = f(x), min (𝑟1,𝑟2) is relative penetration, and δ is penetration; the normal where 𝑥 = spring force is calculated as 𝐹𝑛 = 𝑘𝑒𝑓𝑓 ∙ 𝑦 ∙ 𝑚𝑖𝑛2(𝑟1, 𝑟2) where 𝑘𝑒𝑓𝑓 is the effective bulk modulus of two interacting DEM particles . If curve is defined as 𝑦 = 𝑐 ∙ 𝑥, the behavior is the same as 𝑘1𝑘2 𝑘1+𝑘2 𝑘𝑒𝑓𝑓 = NORMK = c. 3. For two interacting DEMs with user defined curve for shear stiffness y = f(x), where 𝑥 = min (𝑟1,𝑟2) is relative penetration, and δ is penetration; the tangential stiffness is calculated as 𝐾𝑠 = 𝑦 ∙ 𝐾𝑛, where 𝐾𝑛 is norm stiffness defined by NORMK or user defined curve. If curved is defined as y = c, the behavior is the same as SHEARK = c. *CONTROL_DYNAMIC_RELAXATION Purpose: Initialize stresses and deformation in a model to simulate a preload. Examples of preload include load due to gravity, load due to a constant angular velocity, and load due to torquing of a bolt. After the preloaded state is achieved by one of the methods described below, the time resets to zero and the normal phase of the solution automatically begins from the preloaded state. IDRFLG controls the manner in which the preloaded state is computed. If IDRFLG is 1 or -1, a transient “dynamic relaxation” analysis is invoked in which an explicit analysis, damped by means of scaling nodal velocities by the factor DRFCTR each time step, is performed. When the ratio of current distortional kinetic energy to peak distortional kinetic energy (the convergence factor) falls below the convergence tolerance (DRTOL) or when the time reaches DRTERM, the dynamic relaxation analysis stops and the current state becomes the initial state of the subsequent normal analysis. Distortional kinetic energy is defined as total kinetic energy less the kinetic energy due to rigid body motion. A history of the distortional kinetic energy computed during the dynamic relaxation phase is automatically written to a file called “relax”. This file can be read as an ASCII file by LS-PrePost and its data plotted. The “relax” file also includes a history of the convergence factor. To create a binary output database having the same format as a d3plot database but which pertains to the dynamic relaxation analysis, use *DATABASE_BINARY_D3- DRLF. The output interval is given by this command as an integer representing the number of convergence checks between output states. The frequency of the convergence checks is controlled by the parameter NRCYCK. Dynamic relaxation will be invoked if SIDR is set to 1 or 2 in any of the *DEFINE_- CURVE commands, even if IDRFLG = 0 in *CONTROL_DYNAMIC_RELAXATION. Curves so tagged are applicable to the dynamic relaxation analysis phase. Curves with SIDR set to 0 or 2 are applicable to the normal phase of the solution. Dynamic relaxation will always be skipped if IDRFLAG is set to -999. At the conclusion of the dynamic relaxation phase and before the start of the normal solution phase, a binary dump file (d3dump01) and a “prescribed geometry” file (drdisp.sif) are written by LS-DYNA. Either of these files can be used in a subsequent analysis to quickly initialize to the preloaded state without having to repeat the dynamic relaxation run. The binary dump file is utilized via a restart analysis . The drdisp.sif file is utilized by setting IDRFLG=2 as described below and discussed in Remark 1. If IDRFLG is set to 2, the preloaded state is quickly reached by linearly ramping nodal displacements, rotations, and temperatures to prescribed values over 100 time steps, or over a number of time steps as indicated by the variable NC. See the optional cards pertaining to IDRFLG = 2 and also Remarks 1 and 5. If IDRFLG is set to 5, an implicit analysis is performed to obtain the preloaded state and in this case, the preload analysis completes when 'time' is equal to DRTERM. The implicit step size is specified with a *CONTROL_IMPLICIT_GENERAL command. The implicit analysis is, by default, static but can be made transient via the *CONTROL_IM- PLICIT_DYNAMICS command . IDRFLG = 6 also performs an implicit analysis as with IDRFLG = 5 but only for the part subset specified with DRPSET. Card 1 1 2 3 4 5 6 7 8 Variable NRCYCK DRTOL DRFCTR DRTERM TSSFDR IRELAL EDTTL IDRFLG Type I F F F F I F Default 250 0.001 0.995 infinity TSSFAC 0 0.04 I 0 Remarks 3 1, 2, 3 Additional card for IDRFLG = 3 or 6. Card 2 1 2 3 4 5 6 7 8 Variable DRPSET Type Default Remarks I 0 3 4 5 6 7 8 Additional card for IDRFLG = 2. Card 2 Variable 1 NC Type I Default 100 2 NP I 0 NP Additional cards for IDRFLG = 2. Card 3 1 2 3 4 5 6 7 8 Variable PSID VECID Type Default I 0 I 0 VARIABLE NRCYCK DESCRIPTION Number of time steps between convergence checks for explicit dynamic relaxation. DRTOL Convergence (default = 0.001). tolerance for explicit dynamic relaxation DRFCTR Dynamic relaxation factor (default = .995). DRTERM TSSFDR Optional termination time for dynamic relaxation. Termination occurs at this time or when convergence is attained (de- fault = infinity). Scale factor for computed time step during explicit dynamic relaxation. If zero, the value is set to TSSFAC defined on *CON- TROL_TIMESTEP. After converging, the scale factor is reset to TSSFAC. VARIABLE IRELAL DESCRIPTION Automatic control for dynamic relaxation option based on algorithm of Papadrakakis [1981]: EQ.0: not active, EQ.1: active. EDTTL Convergence relaxation. tolerance on automatic control of dynamic IDRFLG Dynamic relaxation flag for stress initialization: EQ.-999: dynamic relaxation not activated even if specified on a load curve, see *DEFINE_CURVE. EQ.-1: dynamic relaxation is activated and time history output is produced during dynamic relaxation, see Remark 2. EQ.0: EQ.1: EQ.2: EQ.3: EQ.5: EQ.6 not active, dynamic relaxation is activated, initialization to a prescribed geometry, see Remark 1, dynamic relaxation is activated as with IDRFLG = 1, but with a part set ID for convergence checking, initialize implicitly, see Remark 3. initialize implicity but only for the part set specified by DRPSET. DRPSET Part set ID for convergence checking (for IDRFLG = 3 or 6 only) NC NP Number of time steps for initializing geometry of IDRFLG = 2. Number of part sets specified for IDRFLG = 2. PSID Part set ID for IDRFLG = 2. VECID Vector ID for defining origin and axis of rotation for IDRFLG = 2. See Remark 5. Remarks: 1. When IDRFLG = 2, an ASCII file specified by "m=" on the LS-DYNA execution line is read which describes the initialized state. The ASCII file contains each node ID with prescribed values of nodal displacement (x, y, z), nodal rotation (x, y, z) and nodal temperature in (I8, 7E15.0) format. 2. If IDRFLG is set to -1 the dynamic relaxation proceeds as normal but time history data is written to the d3thdt file in addition to the normal data being written to the d3drlf file. At the end of dynamic relaxation, the problem time is reset to zero. However, information is written to the d3thdt file with an incre- ment to the time value. The time increment used is reported at the end of dy- namic relaxation. 3. When IDRFLG = 5 or 6, LS-DYNA performs an implicit analysis for the preload phase of the simulation. Parameters for controlling the implicit preload solu- tion are defined using appropriate *CONTROL_IMPLICIT keywords to specify solver type, implicit time step, etc. When using this option, one must specify DRTERM to indicate the termination "time" of the implicit preload analysis. When DRTERM is reached, the implicit preload phase terminates and LS-DY- NA begins the next phase of the analysis according to IMFLAG in *CON- TROL_IMPLICIT_GENERAL. For example, if it is desired to run an implicit preload phase and switch to the explicit solver for the subsequent transient phase, IDRFLG should be set to 5 and IMFLAG should be set to 0. 4. When IDRFLG = 3, a part set ID is used to check for convergence. For example, if only the tires are being inflated on a vehicle, it may be sufficient in some cases to look at convergence based on the part ID’s in the tire and possibly the sus- pension system. You can also use IDRFLG = 6 to perform the initialization using implicit on the part set. 5. When the displacements for IDRFLG = 2 are associated with large rotations, the linear interpolation of the displacement field introduces spurious compression and tension into the part. If a part set is specified with a vector, the displace- ment is interpolated by using polar coordinates with the tail of the vector speci- fying the origin of the coordinate system and the direction specifying the normal to the polar coordinate plane. *CONTROL Purpose: Define controls for the mesh-free computation. Card 1 1 2 3 4 5 6 7 8 Variable ISPLINE IDILA ININT Type Default I 0 I 0 Remarks Card 2 1 2 I 12 1 3 4 5 6 7 8 Variable IMLM ETOL IDEB HSORT SSORT Type Default I 0 F 1.0E-4 I 0 I 0 I 0 VARIABLE DESCRIPTION ISPLINE Optional choice for the mesh-free kernal functions: EQ.0: Cubic spline function (default) EQ.1: Quadratic spline function EQ.2: Cubic spline function with circular disk IDILA Optional choice for the normalized dilation parameter: EQ.0: Maximum distance based on the background element EQ.1: Maximum distance based on surrounding nodes ININT This is the factor needed for the estimation of maximum workspace (MWSPAC) that can be used during the initialization phase. IMLM *CONTROL_EFG DESCRIPTION Optional choice for the matrix operation, linear solving and memory usage: EQ.1: Original BCSLIB-EXT solvers EQ.2: EFGPACK ETOL Error tolerance in the IMLM. When IMLM = 2 is used, ININT in card one becomes redundant. IMLM = 2 is recommended. IDEB Output internal debug message HSORT Not used SSORT Automatic sorting of background triangular shell elements to FEM #2 when EFG shell type 41 is used EQ.0: no sorting EQ.1: full sorting Remarks: 1. The mesh-free computation requires calls to use BCSLIB-EXT solvers during the initialization phase. The maximum workspace (MWSPAC) that can be used during the call is calculated as MWSPAC = ININT3 × NUMNEFG, where NUMNEFG is the total number of mesh-free nodes. ININT, which is the number of nodes that a node influences along each cardinal direction, defaults to 12. When the normalized dilation parameters (DX, DY, DZ) in *SECTION_- SOLID_EFG are increased ININT must likewise increase. 2. When ISPLINE = 2 is used, the input of the normalized dilation parameters (DX, DY, DZ) for the kernel function in *SECTION_SOILD_EFG and SECTI- OL_SHELL_EFG only requires the DX value. 3. EFGPACK was added to automatically compute the required maximum workspace in the initialization phase and to improve efficiency in the matrix operations, linear solving, and memory usage. The original BCSLIB-EXT solver requires an explicit workspace (ININT) for the initialization. *CONTROL Purpose: Provide controls for energy dissipation options. Card 1 1 2 3 4 5 6 7 8 Variable HGEN RWEN SLNTEN RYLEN Type Default I 1 I 2 I 1 I 1 VARIABLE HGEN DESCRIPTION Hourglass energy calculation option. significant additional storage and increases cost by ten percent: This option requires EQ.1: hourglass energy is not computed (default), EQ.2: hourglass energy is computed and included in the energy balance. The hourglass energies are reported in files glstat and matsum, see *DATA- the ASCII BASE_OPTION. RWEN Rigidwall energy (a.k.a. stonewall energy) dissipation option: EQ.1: energy dissipation is not computed, EQ.2: energy dissipation is computed and included in the energy balance (default). The rigidwall energy dissipa- tion is reported in the ASCII file glstat, see *DATA- BASE_OPTION. SLNTEN Sliding interface energy dissipation option (This parameter is always set to 2 if contact is active. The option SLNTEN = 1 is not available.): EQ.1: energy dissipation is not computed, EQ.2: energy dissipation is computed and included in the energy balance. The sliding interface energy is reported in ASCII *DATA- BASE_OPTION. files glstat and sleout, see VARIABLE DESCRIPTION RYLEN Rayleigh energy dissipation option (damping energy dissipation): EQ.1: energy dissipation is not computed (default), EQ.2: energy dissipation is computed and included in the energy balance. The damping energy is reported in *DATA- ASCII BASE_OPTION. and matsum, file glstat see *CONTROL_EXPLICIT_THERMAL The *CONTROL_EXPLICIT_THERMAL_SOLVER keyword activates an explicit finite volume code solving heat transfers by conduction. Enthalpies and temperatures are element centered. The elements supported by the thermal solver are beams, shells, The solids, *CONTROL_EXPLICIT_THERMAL_PROPERTIES keyword defines the heat capacities and conductivities by parts. These 2 keywords are mandatory to properly run the solver. Other keywords can be used to set the initial and boundary conditions and control the outputs. They are all listed below in alphabetical order: multi-material elements. ALE 3D *CONTROL_EXPLICIT_THERMAL_ALE_COUPLING *CONTROL_EXPLICIT_THERMAL_BOUNDARY *CONTROL_EXPLICIT_THERMAL_CONTACT *CONTROL_EXPLICIT_THERMAL_INITIAL *CONTROL_EXPLICIT_THERMAL_OUTPUT *CONTROL_EXPLICIT_THERMAL_PROPERTIES *CONTROL_EXPLICIT_THERMAL_SOLVER *CONTROL_EXPLICIT_THERMAL_ALE_COUPLING Purpose: Define the shell and solid parts involved in an explicit finite volume thermal requires coupling with multi-material ALE *CONSTRAINED_LAGRANGE_IN_SOLID, CTYPE = 4. keyword groups. This Card 1 1 2 3 4 5 6 7 8 Variable PARTSET MMGSET Type I I Default none none VARIABLE DESCRIPTION PARTSET Part set ID MMGSET Multi-material MATERIAL_GROUP_LIST) set ID (see *SET_MULTI- Remarks: *CONTROL_EXPLICIT_THERMAL_BOUNDARY Purpose: Set temperature boundaries with segment sets for an explicit finite volume thermal analysis. Card 1 1 2 3 4 5 6 7 8 Variable SEGSET LCID Type I F Default none none VARIABLE DESCRIPTION SEGSET Segment set ID LCID *DEFINE_CURVE ID defining the temperature in function of time Remarks: 1. Boundary elements. The boundary temperatures are set at segment centers. If shells or beams have all their nodes in the segment set, these elements would be considered as boundary elements: the temperatures at their centers will be controlled by the curve LCID. *CONTROL_EXPLICIT_THERMAL_CONTACT Purpose: Define the beam, shell and solid parts involved in an explicit finite volume thermal contact. Card 1 1 2 3 4 5 6 7 8 Variable PARTSET NCYCLE Type I Default none F 1 VARIABLE DESCRIPTION PARTSET Part set ID NCYCLE Number of cycle between checks of new contact Remarks: *CONTROL_EXPLICIT_THERMAL_INITIAL Purpose: Initialize the temperature centered in beams, shells or solids involved in an explicit finite volume thermal analysis. Card 1 1 2 3 4 5 6 7 8 Variable SET SETYP TEMPINI Type I F F Default none none 0.0 VARIABLE DESCRIPTION SET set ID SETYP Type of set: EQ.1: solid set EQ.2: shell set EQ.3: TEMPINI Initial temperature Remarks: 1. Material with *EOS. The volumetric enthalpy is the sum of the pressure and volumetric internal energy (as defined in *EOS). If the material has an equation of state, the enthalpy should not be initialized by the temperature but by the initial volumetric internal energy and pressure set in *EOS. *CONTROL_EXPLICIT_THERMAL_OUTPUT Purpose: Output temperatures and enthalpies for an explicit finite volume thermal analysis. Card 1 1 2 3 4 5 6 7 8 Variable DTOUT DTOUTYP SET SETYP Type F Default none I 0 I 0 I 0 VARIABLE DESCRIPTION DTOUT Time interval between outputs DTOUTYP Type of DTOUT: EQ.0: DTOUT is a constant EQ.1: DTOUT is the ID of *DEFINE_CURVE defining a table of time vs DTOUT SET set ID SETYP Type of set: EQ.1: solid set EQ.2: shell set EQ.3: beam set . 2. Output by element. If a set of elements SET is defined, the temperature and enthalpy histories are output by element in a .xy format. The file names are and temperature_{beam,shell,solid}ID.xy The binary file xplcth_output is not output. enthalpy_{beam,shell,solid}ID.xy. *CONTROL_EXPLICIT_THERMAL_PROPERTIES Purpose: Define the thermal properties of beam, shell and solid parts involved in an explicit finite volume thermal analysis. Card 1 1 2 3 4 5 6 7 8 Variable PARTSET CP CPTYP VECID1 VECID2 LOCAL Type I F Default none none Card 2 1 2 I 0 3 I 0 4 I 0 5 I 0 6 Variable Kxx Kxy Kxz KxxTYP KxyTYP KxzTYP Type F F F Default 0.0 0.0 0.0 Card 3 1 2 3 I 0 4 I 0 5 I 0 6 Variable Kyx Kyy Kyz KyxTYP KyyTYP KyzTYP Type F F F Default 0.0 0.0 0.0 I 0 I 0 I 0 7 8 7 Card 4 1 2 3 4 5 6 7 8 Variable Kzx Kzy Kzz KzxTYP KzyTYP KzzTYP Type F F F Default 0.0 0.0 0.0 I 0 I 0 I 0 VARIABLE DESCRIPTION PARTSET Part set ID CP Heat capacity CPTYP Type of CP: EQ.0: CP is a constant VECID1, VECID2 EQ.1: CP is the ID of *DEFINE_CURVE defining a table of temperature vs heat capacity *DEFINE_VECTOR IDs to define a specific coordinate system. VECID1 and VECID2 give the 𝑥- and 𝑦-direction respectively. The 𝑧-vector is a cross product of VECID1 and VECID2. If this latter is not orthogonal to VECID1, its direction will be corrected with a cross-product of 𝑧- and 𝑥-vectors. The conductivity matrix Kij is applied this coordinate system. LOCAL Flag to activate an element coordinate system: EQ.0: The vectors VECIDj are considered in a global coordinate system. EQ.1: The vectors VECIDj are considered in a local system attached to the element. For shells and solids, the system is the same as DIREC = 1 and CTYPE = 12 in *CON- STRAINED_LAGRANGE_IN_SOLID. For shells, the edge centers replace the face centers. For beams, the 𝑥- in direction *ELEMENT_BEAM and there should be a 3rd node for the 𝑦-direction. is aligned with first 2 nodes the Kij Heat conductivity matrix VARIABLE DESCRIPTION KijTYP Type of Kij: EQ.0: Kij is a constant EQ.1: Kij is the ID of *DEFINE_CURVE defining a table of temperature vs heat conductivity Remarks: *CONTROL_EXPLICIT_THERMAL_SOLVER Purpose: Define the beam, shell and solid parts involved in a finite volume thermal analysis. The enthalpies and temperatures are explicitly updated in time. Card 1 1 2 3 4 5 6 7 8 Variable PARTSET DTFAC Type I F Default none 1.0 VARIABLE DESCRIPTION PARTSET Part set ID DTFAC Time step factor Remarks: 1. Time step. The time step is a minimum of the mechanical and thermal time steps. The thermal time step is a minimum of the element thermal time steps, which are half the enthalpies divided by the right hand side of the heat equa- tion (conductivity * temperature laplacian). The thermal time step is scaled by DTFAC (=1 by default) *CONTROL_EXPLOSIVE_SHADOW_{OPTION} Available option includes: <BLANK> SET Purpose: Compute detonation times in explosive elements for which there is no direct line of sight. If this command is not included in the input, the lighting time for an explosive element is computed using the distance from the center of the element to the nearest detonation point, 𝐿𝑑; the detonation velocity, 𝐷; and the lighting time for the detonator, 𝑡𝑑: 𝑡𝐿 = 𝑡𝑑 + 𝐿𝑑 The detonation velocity for this option is taken from the element whose lighting time is computed and does not account for the possibilities that the detonation wave may travel through other explosives with different detonation velocities or that the line of sight may pass outside of the explosive material. If this command is present, the lighting time of each explosive element is based on the shortest path through the explosive material from the associated detonation point(s) to the explosive element. If inert obstacles exist within the explosive material, the lighting time will account for the extra time required for the detonation wave to travel around the obstacles. The lighting times also automatically accounts for variations in the detonation velocity if different explosives are used. The SET option requires input of a set ID of two-dimensional shell elements or three- dimensional solid elements for which explosive shadowing is active. If the SET option is not used, Card 1 should be omitted and shadowing is active for all explosive elements. See also *INITIAL_DETONATION and *MAT_HIGH_EXPLOSIVE. Card 1. Card for SET keyword option. Card 1 1 2 3 4 5 6 7 8 Variable SETID Type I Default None VARIABLE SETID DESCRIPTION Set ID of a *SET_SHELL or *SET_SOLID. If the SET option is active, the lighting times are computed for a set of shells (*SET_SHELL in two dimensions) or solids (*SET_SOLID in three dimensions). *CONTROL_FORMING Purpose: Set parameters for metal forming related features. *CONTROL_FORMING_AUTOCHECK *CONTROL_FORMING_AUTO_NET *CONTROL_FORMING_AUTOPOSITION *CONTROL_FORMING_BESTFIT *CONTROL_FORMING_INITIAL_THICKNESS *CONTROL_FORMING_MAXID *CONTROL_FORMING_ONESTEP *CONTROL_FORMING_OUTPUT *CONTROL_FORMING_PARAMETER_READ *CONTROL_FORMING_POSITION *CONTROL_FORMING_PRE_BENDING *CONTROL_FORMING_PROJECTION *CONTROL_FORMING_REMOVE_ADAPTIVE_CONSTRAINTS *CONTROL_FORMING_SCRAP_FALL *CONTROL_FORMING_SHELL_TO_TSHELL *CONTROL_FORMING_STONING *CONTROL_FORMING_TEMPLATE *CONTROL_FORMING_TIPPING *CONTROL_FORMING_TOLERANC *CONTROL_FORMING_TRAVEL *CONTROL_FORMING_TRIM_MERGE *CONTROL_FORMING_TRIMMING *CONTROL_FORMING_UNFLANGING *CONTROL_FORMING_USER *CONTROL_FORMING_AUTOCHECK Purpose: This keyword detects and corrects flaws in the mesh for the rigid body that models the tooling. Among its diagnostics are checks for duplicated elements, overlapping elements, skinny/long elements, degenerated elements, disconnected elements, and inconsistent element normal vectors. This feature also automatically orients each tool’s element normal vectors so that they face the blank. Additionally an offset can be specified to create another tool (tool physical offset) based on the corrected tool meshes. Note that this keyword is distinct from *CONTROL_CHECK_SHELL, which checks and corrects mesh quality problem after trimming, to prepare the trimmed mesh for the next stamping process. This keyword only applies to shell elements. The tool offset feature is now available in LS-PrePost 4.2 under Application → MetalForming → Easy Setup. Card 1 1 2 3 4 5 6 7 8 Variable ICHECK IGD IOFFSET IOUTPUT Type Default I 0 I none I 0 I none VARIABLE DESCRIPTION ICHECK Tool mesh checking/correcting flag: ICHECK.EQ.0: Do not activate mesh checking/correcting feature. ICHECK.EQ.1: Activate comprehensive mesh check and correct problematic tool meshes . This option reduces the likelihood of unreason- able forming results and/or error termination. This is only for regular forming simulations. The calculation will continue after the tool mesh checking/correcting phase is completed. See Example 1. The corrected tool meshes can be viewed and recovered from the resulting d3plot files. If the termination time is set to “0.0” or the keyword *CONTROL_TERMINATION is absent all to- gether, the simulation will terminate as soon as checking/correcting is completed, and correct- ed tool meshes can be extracted from the d3plot files. IGD Not used. IOFFSET Tool mesh offset flag. This variable works only when IOUTPUT is defined, and ICHECK is set to “1”: IOFFSET.EQ.0: Do not offset rigid tool mesh. The sheet blank does not need to be present. In this case the output files rigid_offset.inc and rigid_offset_ before.inc will be identical. See Example 2. IOFFSET.EQ.1: Perform rigid tool mesh offset using the variable MST as specified on a *CONTACT_FORMING_… card. The blank must be defined and positioned completely above or below the rigid tool to be offset. Both part ID and part SID (MSTYP) can be used in defining the MSID. IOUTPUT must also be de- fined. VARIABLE DESCRIPTION IOUTPUT Output option flag: IOUTPUT.EQ.1: Output offset rigid tool meshes into a keyword file rigid_offset.inc, and terminates the simula- tion. IOUTPUT.EQ.2: Output offset rigid tool meshes as well as nodes used to define draw beads into a key- word file rigid_offset.inc, and terminates the simulation. See Example 4. IOUTPUT.EQ.3: Output checked/corrected tool as well as offset rigid tool meshes into two separate key- word files, rigid_offset_before.inc, and rigid_ offset.inc, respectively, and terminates the simulation. See Example 3. IOUTPUT.EQ.4: Output checked/corrected tool meshes, offset rigid tool meshes as well as the nodes used to define draw beads into two separate keyword rigid_ files, offset.inc, respectively, and terminates the simulation. rigid_offset_before.inc, and Remarks: In sheet metal forming, tools are typically modelled as rigid bodies and their meshes are prepared from CAD (IGES or STEP) files according to the following procedure: 1. The user imports the CAD data into a preprocessor, such as LS-PrePost. 2. The preprocessor automatically generates a mesh. LS-PrePost features a streamlined GUI for this application. 3. Export the generated mesh to LS-DYNA input files. The LS-PrePost eZ-Setup user interface provides quick access to generate the necessary input files for metal forming applications. Ideally, this process should produce a good mesh requiring no manual intervention. Often, though, such meshes that have been automatically generated from CAD data have flaws severe enough to prevent an accurate or complete calculation. This feature, *CONTROL_FORMING_AUTOCHECK is intended to make LS-DYNA more robust with respect to tooling mesh quality. This keyword requires that the tooling meshes represent rigid bodies. Also, when this keyword is used, a part ID or a part set ID, corresponding to MSTYP = 2 or 3 on the *CONTACT_FORMING_… card, may be used to define the master side, MSID. Segment set ID input, MSTYP = 0, is not supported. Some cases of incoming bad tooling meshes which can be corrected by this keyword are shown in Figure 12-15. This keyword can be inserted anywhere in the input deck. To include the corrected tooling mesh into the d3plot the ICHECK field must be defined. The corrected mesh is written to rigid_offset_before.inc file if IOFFSET and IOUTPUT are defined. When IOFFSET = 1 and IOUTPUT is defined, the tool meshes will first be checked, corrected, and reoriented correctly towards the blank. Then the tool is offset by an amount of 0.5|MST| either on the same or opposite side of the blank, depending on the signs of the MST field on the *CONTACT_FORMING_… card (Figure 12-14). A new keyword file, “rigid_offset.inc” file, will be output as containing the corrected, reoriented, and offset tooling mesh. The tool offset feature is now available in LS-PrePost 4.2 under Application → MetalForming → Easy Setup. The offset from Die button under Binder can be used to create offset tools. Note this keyword does not work with the SMOOTH option in *CONTACT_FORM- ING_… prior to Revision 95456, see Revision information. Example 1 - Mesh checking/correction in a regular forming simulation: The keyword can be inserted anywhere in a regular forming simulation input deck. A partial input example of checking, correcting the tool meshes and reorienting all tools’ normals is provided below. Note that although MST is defined between blank and die contact interface, die meshes will not be offset, since IOFFSET is not defined. Simulation will continue if “&endtime” is not zero, but will terminate as soon as the checking and correcting are done if “&endtime” is set to “0.0”, or *CONTROL_TERMI- NATION is absent all together. Corrected and reoriented tool meshes can be viewed and recovered from d3plot files. *KEYWORD *INCLUDE Tool_blank.k *CONTROL_FORMING_AUTOCHECK $ ICHECK IGD IOFFSET IOUTOUT 1 *CONTROL_TERMINATION &endtime ⋮ *CONTACT_FORMING_ONE_WAY_SURFACE_TO_SURFACE_ID 1 blank to punch 1 2 2 2 1 1 0.110E+00 0.000E+00 0.000E+00 0.000E+00 0.200E+02 0.0000E+00 0.100E+21 0.000 0.000 0.0 *CONTACT_FORMING_ONE_WAY_SURFACE_TO_SURFACE_ID 2 blank to die $ SSID MSID SSTYP MSTYP SBOXID MBOXID SPR MPR 1 3 2 2 1 1 $ FS FD DC VC VDC PENCHK BT DT 0.110E+00 0.000E+00 0.000E+00 0.000E+00 0.200E+02 0.000E+00 0.100E+21 $ SFS SFM SST MST SFST SFMT FSF VSF 0.000 0.000 -1.600 $ SOFT SOFSCL LCIDAB MAXPAR PENTOL DEPTH BSORT FRCFRQ 0 *CONTACT_FORMING_ONE_WAY_SURFACE_TO_SURFACE_ID 3 blank to binder 1 4 2 2 1 1 0.110E+00 0.000E+00 0.000E+00 0.000E+00 0.200E+02 0.000E+00 0.100E+21 0.000 0.000 0.0 ⋮ *END Example 2 - Mesh checking/correction only for rigid tool mesh (sheet blank not required): A much shorter but complete input example of checking, correcting the tool meshes and reorienting all tools’ normals is shown below. Note the sheet blank does not need to be present, and both rigid_offset.inc and rigid_offset_before.inc will be the same, representing the checked, corrected, and reoriented tool mesh file, since IOFFSET is undefined (no tool offset will be done). *KEYWORD *INCLUDE toolmesh.k *CONTROL_FORMING_AUTOCHECK $ ICHECK IGD IOFFSET IOUTOUT 1 1 *PARAMETER_EXPRESSION I toolpid 3 *PART $ PID SECID MID EOSID HGID GRAV ADPOPT TMID &toolpid 2 2 *MAT_RIGID $ MID RO E PR N COUPLE M ALIAS 2 7.83E-09 2.07E+05 0.28 $ CMO CON1 CON2 1 4 7 $LCO or A1 A2 A3 V1 V2 V3 *SECTION_SHELL $ SECID ELFORM SHRF NIP PROPT QR/IRID ICOMP SETYP 2 2 1.0 3.0 0.0 $ T1 T2 T3 T4 NLOC 1.0 1.0 1.0 1.0 *END Example 3 - Mesh checking/correction and tool offset (sheet blank required): In addition to checking, correcting and reorienting all tools’ normal, the following partial input will offset the die meshes in toolmesh.k by 0.88 mm (using the MST value defined for the die) on the opposite side of the blank, and output the offset tool meshes in a file rigid_offset.inc. The checked/corrected original die meshes will be written to rigid_offset_before.inc. The simulation will terminate as soon as the files are written, regardless of what the “&endtime” value is. In fact, the keyword *CONTROL_TERMI- NATION can be omitted all together. *KEYWORD *INCLUDE Tool_blank.k *PARAMETER_EXPRESSION R blankt 0.8 R offset -1.1 R mst blankt*offset*2.0 *CONTROL_FORMING_AUTOCHECK $ ICHECK IGD IOFFSET IOUTOUT 1 1 3 *CONTROL_TERMINATION &endtime *CONTACT_FORMING_ONE_WAY_SURFACE_TO_SURFACE_ID 1 blank to punch 1 2 2 2 1 1 0.110E+00 0.000E+00 0.000E+00 0.000E+00 0.200E+02 0.0000E+00 0.100E+21 0.000 0.000 0.0 *CONTACT_FORMING_ONE_WAY_SURFACE_TO_SURFACE_ID 2 blank to die $ SSID MSID SSTYP MSTYP SBOXID MBOXID SPR MPR 1 3 2 2 1 1 $ FS FD DC VC VDC PENCHK BT DT 0.110E+00 0.000E+00 0.000E+00 0.000E+00 0.200E+02 0.000E+00 0.100E+21 $ SFS SFM SST MST SFST SFMT FSF VSF 0.000 0.000 &mst $ SOFT SOFSCL LCIDAB MAXPAR PENTOL DEPTH BSORT FRCFRQ 0 *CONTACT_FORMING_ONE_WAY_SURFACE_TO_SURFACE_ID 3 blank to binder 1 4 2 2 1 1 0.110E+00 0.000E+00 0.000E+00 0.000E+00 0.200E+02 0.000E+00 0.100E+21 0.000 0.000 0.0 *END Example 4 - Mesh checking/correction and tool offset, bead nodes output (sheet blank required): In addition to checking, correcting and reorienting all tools’ normal, the following partial input will create an offset tool in the file rigid_offset.inc on the same side of the blank; the file will also contain the nodes used to define the contact draw beads #1 and #2. *KEYWORD *INCLUDE Tool_blank.k R blankt 0.8 R offset 1.1 R mst blankt*offset*2.0 *CONTROL_FORMING_AUTOCHECK $ ICHECK IGD IOFFSET IOUTOUT 1 1 2 *CONTROL_TERMINATION &endtime *CONTACT_FORMING_ONE_WAY_SURFACE_TO_SURFACE_ID 1 blank to punch 1 2 2 2 1 1 0.110E+00 0.000E+00 0.000E+00 0.000E+00 0.200E+02 0.0000E+00 0.100E+21 0.000 0.000 0.0 *CONTACT_FORMING_ONE_WAY_SURFACE_TO_SURFACE_ID 2 blank to die $ SSID MSID SSTYP MSTYP SBOXID MBOXID SPR MPR 1 3 2 2 1 1 $ FS FD DC VC VDC PENCHK BT DT 0.110E+00 0.000E+00 0.000E+00 0.000E+00 0.200E+02 0.000E+00 0.100E+21 $ SFS SFM SST MST SFST SFMT FSF VSF 0.000 0.000 &mst $ SOFT SOFSCL LCIDAB MAXPAR PENTOL DEPTH BSORT FRCFRQ 0 *CONTACT_FORMING_ONE_WAY_SURFACE_TO_SURFACE_ID 3 blank to binder 1 4 2 2 1 1 0.110E+00 0.000E+00 0.000E+00 0.000E+00 0.200E+02 0.000E+00 0.100E+21 0.000 0.000 0.0 ⋮ *CONTACT_DRAWBEAD_ID 10001 Draw bead #1 1 1 4 2 0 0 0 0.110E+00 0.000E+00 0.000E+00 0.000E+00 0.200E+00 0.0615 0.100E+21 0.200 0.200 $ LCIDRF LCIDNF DBDTH DFSCL NUMINT 10 9 0.100E+02 0.700E+00 *CONSTRAINED_EXTRA_NODES_SET 40 1 *SET_NODE_LIST 1 915110 915111 915112 915113 915114 915115 915116 915117 915118 915119 915120 915121 915122 *CONTACT_DRAWBEAD_ID 10002 Draw bead #2 2 1 4 2 0 0 0 0.110E+00 0.000E+00 0.000E+00 0.000E+00 0.200E+00 0.0615 0.100E+21 0.200 0.200 $ LCIDRF LCIDNF DBDTH DFSCL NUMINT 11 9 0.100E+02 0.400E+00 *CONSTRAINED_EXTRA_NODES_SET $ PID NSID 40 2 *SET_NODE_LIST 2 915123 915124 915125 915126 915127 915128 915129 915130 915131 915132 915133 915134 915135 915136 915137 ⋮ *END Revision information: This feature is available starting from LS-DYNA Revision 91737, in both SMP, MPP and double precision. 1. 2. IOFFSET, and IOUTPUT = 1 are available starting in Revision 94521. The latest beta revisions should offer better and improved offset meshes. IOUTPUT = 2 is available starting in Revision 95357. 3. Support of SMOOTH contact option in *CONTACT_FORMING...: is available starting in Revision 95456. 4. IOUTPUT = 3, and 4 are available starting in Revision 96592. Sheet metal blank must be positioned completely above or below the original tool Original tool (corrected original tool in rigid_offset_before.inc) A negative MST result in a new tool with normal offset distance |(0.5)MST| from the original tool, on the opposite side of the blank Offset tool (rigid_offset.inc) Sheet metal blank must be positioned completely above or below the original tool Offset tool (rigid_offset.inc) A positive MST result in a new tool with normal offset distance |(0.5)MST| from the original tool, on the same side of the blank Original tool (corrected original tool in rigid_offset_before.inc) Figure 12-14. Offset using the MST value defined in *CONTACT_- FORMING_… All nodes of two duplicate traingle shells 21304, 34630 lie in one straight line Shell 34608 overlaps with three other triangle shells Overlapping shell 34604 Overlapping shell 34607 A severe, multiple overlapping case A case of typical incoming, inconsistent shell normals Figure 12-15. A few cases of the tooling mesh problems handled by this keyword. *CONTROL_FORMING_AUTO_NET Purpose: This keyword is used for simulating springback when the stamping panel is resting on the nets of a checking fixture. With this keyword, rectangular nets are automatically generated according to specified dimensions and positions. Include one pair of Cards 1 and 2 per net. Add to the deck as many pairs of cards as needed. This section is terminated by the next keyword (“*”) card. In general, for N nets add 2N cards. 4 IDP I 0 4 8 5 X F 6 Y F 7 Z F 0.0 0.0 0.0 5 6 7 8 Card 1 1 2 3 Variable IDNET ITYPE IDV Type I Default none Card 2 Variable 1 SX Type F 2 SY F I 0 3 OFFSET F Default 0.0 0.0 0.0 VARIABLE DESCRIPTION IDNET ID of the net; must be unique. ITYPE Not used at this time. IDV Vector ID for surface normal of the net. See *DEFINE_VECTOR. If not defined, the normal vector will default to the global z-axis. IDP Part ID of the panel undergoing springback simulation. X Y The x-coordinate of a reference point for the net to be generated. The y-coordinate of a reference point for the net to be generated. VARIABLE DESCRIPTION Z SX SY The z-coordinate of a reference point for the net to be generated. Length of the net along the first tangential direction. (The x-axis when the normal is aligned along the global z-axis). Length of the net along the second tangential direction. (The y- axis when the normal is aligned along the global z-axis). OFFSET The net center will be offset a distance of OFFSET in the direction of its surface normal. For positive values, the offset is parallel to the normal; for negative values, antiparallel. General remarks: 1. The IDNET field of card 1 sets the “net ID,” which is distinct from the part ID of the net; the net ID serves distinguishes this net from other nets. 2. The part ID assigned to the net is generated by incrementing the largest part ID value in the model. 3. Other properties such as section, material, and contact interfaces between the panel and nets are likewise automatically generated. 4. The auto nets use contact type *CONTACT_FORMING_ONE_WAY_SUR- FACE_TO_SURFACE. An example: The excerpted input file specifies four auto nets having IDs 1 through 4. The vector with ID = 89 is normal to the net. The nets are offset 4 mm below their reference points; the direction is below because the normal vector (ID = 89) is parallel to the z-axis and the offset is negative. This example input can be readily adapted to a typical gravity-loaded springback simulation obviating the need for SPC constraints . *CONTROL_FORMING_AUTO_NET $---+----1----+----2----+----3----+----4----+----5----+----6----+----7----+----8 $ IDNET ITYPE IDV IDP X Y Z 1 89 5 2209.82 -33.6332 1782.48 $ SX SY OFFSET 15.0 15.0 -4.0 $ IDNET ITYPE IDV IDP X Y Z 2 89 5 3060.23 -33.6335 1782.48 $ SX SY OFFSET 15.0 15.0 -4.0 $ IDNET ITYPE IDV IDP X Y Z 3 89 5 3061.21 31.4167 1784.87 $ SX SY OFFSET Nets automatically generated Two specified coordinate locations Trimmed panel Figure 12-16. An example problem. 15.0 15.0 -4.0 $ IDNET ITYPE IDV IDP X Y Z 4 89 5 2208.84 31.4114 1784.87 $ SX SY OFFSET 15.0 15.0 -4.0 *DEFINE_VECTOR $ VID, Tail X, Y, Z, Head X, Y, Z 89,0.0,0.0,0.0,0.0,0.0,100.0 Discussion of Figures: Figure 12-16 shows a formed and trimmed panel of a hat-shaped channel with an auto net at two corners. The nets are offset 4mm away from the panel. When gravity loading is downward the nets must be below the panel (Figure 12-17 left) so that the panel comes into contact with the nets after springback as expected (Figure 12-17 right). As shown in Figure 12-18 the situation must be reversed when gravity loading points upward. Revision information: This feature is now available starting in implicit static in double precision LS-DYNA Revision 62781. Initial OFFSET 4mm with gravity load down Before springback After springback Figure 12-17. Springback and contact with nets - gravity down. Initial OFFSET 4mm with gravity load up Before springback After springback Figure 12-18. Springback and contact with nets – gravity up. *CONTROL_FORMING_AUTOPOSITION_PARAMETER_{OPTION} Available options include: <BLANK> SET Purpose: The purpose of this keyword is to calculate the minimum required separation distances among forming tools for initial tool and blank positioning in metal forming simulation. It is applicable to shell elements only. It does not, actually, move the part; for that, see *PART_MOVE. NOTE: This keyword requires that model begin in its home position. While processing this card, LS-DYNA moves the parts to match the auto-position results so that auto-position operations correctly compose. Upon completion of the auto-positioning phase, the parts are returned to their home positions. Auto-Position Part Cards. Add one card for each part to be auto-positioned. The next keyword (“*”) card terminates this is keyword. Card 1 1 2 3 4 5 6 7 8 Variable PID CID DIR MPID POSITION PREMOVE THICK PORDER Type I Default none I 0 I I none none I 0 F F I/A 0.0 0.0 none VARIABLE PID DESCRIPTION Part ID. This part will be moved based on the following controlling parameters. When the option SET is activated, PID becomes part set ID, defined by *SET_PART_LIST. This is useful in defining tailor- welded blanks, where two pieces of the blank must be moved simultaneously. CID Coordinate ID (Default is global coordinate system). VARIABLE DESCRIPTION DIR Direction in which the part will be moved: EQ.1: x direction, EQ.2: y direction, EQ.3: z direction. MPID Master part ID, whose position is to be referenced by PID for positioning. When the option SET is activated, MPID becomes part set ID, defined by *SET_PART_LIST. POSITION Definition of relative position between PID and MPID: EQ.1: PID is above MPID; EQ.-1: PID is below MPID. Definition of “above” is determined by the defined coordinate system. If PID is above MPID, it means PID has a larger z- coordinate. This definition is helpful in line die simulation where local coordinate system may be used. Move PID through distance PREMOVE prior to processing the other *CONTROL_FORMING_AUTOPOSITION cards. See Remark 5. Thickness of the blank. The same value must be used in all defined move operations under this keyword. The name of the parameter without the ampersand “&”, as defined in *PARAMETER, or the position or order of the parameter defined in the *PARAMETER list. PREMOVE THICK PORDER Background: In line-die (multi-stage) simulation, initial positioning of the tools and blank is one of the major issues preventing several die processes from being run automatically from a single job submission. The most basic method for running a line die simulation is to chain a series of calculations together using the previous calculation’s partially formed blank, written to a dynain file, as a part of the input for the next calculation. Since the partial results are not known until the preceding calculation completes, the tools need to reposition before the next calculation. Without this card the repositioning step must be done by-hand using a preprocessor. With the combination of this card and the LS-DYNA case driver the repositioning can be fully automated, enabling a complete line-die simulation to be completed with a single job submission. *CONTROL_FORMING_AUTOPOSITION_PARAMETER This card requires that all parts start in their home (tool closed) position. It calculates how far the parts need to be moved to prevent initial penetration. The results are stored into the parameter listed in the PORDER field to be used for a part move operation. 1. For each defined move operation a *PARAMETER card must initialize the parameter referred to in the PORDER field. 2. All tools must start in home position including desired final gaps. 3. The required distance between each contact pair is calculated and stored in the initialized parameter named in the PORDER field. 4. The parts are repositioned through a distance based on the value written to the parameter PORDER using the *PART_MOVE card. 5. The *PARAMETER_EXPRESSION can be used to evaluate expressions depending on the move distances, such as times and tool move speeds. 6. The *CASE feature, is used to chain together the sub-processes in the line-dime simulation. Remarks: 1. Order Dependence. Input associated with this keyword is order sensitive. The following order should be observed: a) All model information including all elements and node b) Part definitions c) Part set definitions d) *PARAMETER initialization e) This keyword f) *PARAMETER_EXPRESSION g) *PART_MOVE 2. This keyword can also be used to generate a new keyword input (dynain) containing the fully positioned model (without actually running the entire simulation). This procedure is identical to a full calculation except that the *PA- RAMETER_EXPRESSION keyword, the *CONTROL_TERMINATION key- word, and tool kinematic definitions are omitted. 3. When working in local coordinate systems it is often the case that the sign of the computed parameter may not correspond to its intended use. In this case, the absolute value function, ABS, for the *PARAMETER_EXPRESSION key- word is especially useful. 4. Draw beads can be modeled with beam elements that are positioned and attached to a tool at home position. Draw beads with beam elements can also be moved in the keyword *PART_MOVE, and automatically positioned just like any other types of elements. 5. Cards with the PREMOVE field set are processed before all other *CONTROL_- FORMING_AUTOPOSITON cards, regardless of their location in the input deck. The PREMOVE field serves to modify the initial state on which the calcu- lations of the other AUTOPOSITON cards are based. For instance, when a binder is moved downward with the PREMOVE feature, it will be in its post-PREMOVE position for all other AUTOPOSITION calcula- tions. But, as is the case with the other AUTOPOSITON cards, the model will be returned to its home position upon completion of the AUTOPOSITION phase. Note that the master part, MPID, and the POSITION fields are ignored when the PREMOVE field is set, and that the PREMOVE value is copied into the PORDER parameter. 6. This feature is implemented in LS-PrePost4.0 eZSetup (http://ftp.lstc.com/- anonymous/ outgoing/lsprepost/4.0/metalforming/) for metal forming in both explicit and implicit application. Part set 2 (lower binder) Part set 1 (blank) Part set 3 (upper die) Binder PREMOVE (183.0 mm) Initial position (tools home) Final position (after auto-position) Figure 12-19. An example of using the variable PREMOVE Example 1: An air draw process like the one shown in Figure 12-19 provides a clear illustration of how this card, and, in particular, the PREMOVE field is used to specify the lower binder’s travel distance. 1. The card with the PREMOVE field set, the third AUTOPOSITON card, is processed first. It moves lower binder 183 mm upward from its home position, and it will form the base configuration for other AUTOPOSITION cards. It will also store this move into &bindmv. Note that although the POSITION and MPID fields are set, they are ignored. 2. The first autoposition card, which will be the second one processed, calculates the minimum offset distance (&blankmv) necessary for the blank (part set 1) to clear part set 9999, which consists of the lower binder (PID = 2), which is in its post-PREMOVE location, and of the lower punch (PID = &lpunid). 3. The next card determines the minimum offset (&updiemv) necessary to bring the upper die (part set 3) as close to the blank as possible without penetrating. This calculation proceeds under the assumption that the blank part set has been moved through &blankmv. *SET_PART_LIST 9999 &lpunpid,2 $---+----1----+----2----+----3----+----4----+----5----+----6----+----7----+----8 *CONTROL_FORMING_AUTOPOSITION_PARAMETER_SET $---+----1----+----2----+----3----+----4----+----5----+----6----+----7----+----8 $ PID CID DIR MPID POSITION PREMOVE THICK PORDER $ blank move 1 3 9999 1 &bthick blankmv $ upper die move 3 3 1 1 &bthick updiemv $ lower binder move 2 3 1 -1 183.0 &bthick bindmv $---+----1----+----2----+----3----+----4----+----5----+----6----+----7----+----8 *PART_MOVE $ SID XMOV YMOV ZMOV CID IFSET $ blank move 1 0.0 0.0 &blankmv 1 $ upper die move 3 0.0 0.0 &updiemv 1 $ lower binder move 2 0.0 0.0 &bindmv 1 The following examples demonstrates the *PARAMETER_EXPRESSION card, which is used to derive new parameters from the value calculated during auto-positioning. In this example, the auto-positioned distance for binder, which is stored in the parameter, &bindmv, is used to define an additional parameter, &bindmv1 = &bindmv − 30 mm The *PART_MOVE step uses &bindmv1 rather than &bindmv, to move both the lower binder and the draw beads. $---+----1----+----2----+----3----+----4----+----5----+----6----+----7----+----8 *CONTROL_FORMING_AUTOPOSION_PARAMETER_SET $---+----1----+----2----+----3----+----4----+----5----+----6----+----7----+----8 $ PID CID DIR MPID POSITION PREMOVE THICK PORDER $ blank move &blksid 3 9999 1 &bthick blankmv $ upper die move &udiesid 3 &blksid 1 &bthick updiemv $ lower binder move &bindsid 3 &blksid -1 &bthick bindmv $---+----1----+----2----+----3----+----4----+----5----+----6----+----7----+----8 *PARAMETER_EXPRESSION bindmv1 bindmv-30.0 $---+----1----+----2----+----3----+----4----+----5----+----6----+----7----+----8 *PART_MOVE $ SID XMOV YMOV ZMOV CID IFSET $ blank move &blksid 0.0 0.0 &blankmv 1 $ upper die move &udiesid 0.0 0.0 &updiemv 1 $ lower binder move &bindsid 0.0 0.0 &bindmv1 1 $ draw beads move 909 0.0 0.0 &bindmv1 1 Part set 2 (upper die) Part set 1 (blank) &updiemv &updiemv &blankmv &blankmv Part set 3 (lower binder) Figure 12-20. An example of binder closing in air draw Example 2: Figure 12-20 schematically shows the binder closing in the global Z-direction. A partial keyword details follow. *INCLUDE $blank from previous case case5.dynain *INCLUDE closing_tool.k *INCLUDE beads_home.k *SET_PART_LIST $ blank 1 1 *SET_PART_LIST $ upper die 2 2 *SET_PART_LIST $ lower binder 3 3 $---+----1----+----2----+----3----+----4----+----5----+----6----+----7----+----8 *parameter $$$$$$$$$$$$$$$$$$$$$$$$$$ Tool move variables R blankmv 0.0 R updiemv 0.0 R bindmv 0.0 $$$$$$$$$$$$$$$$$$$$$$$$$$ Tool speed and ramp up definition R tclsup 0.001 R vcls 1000.0 $---+----1----+----2----+----3----+----4----+----5----+----6----+----7----+----8 *CONTROL_FORMING_AUTOPOSION_PARAMETER_SET $ PID CID DIR MPID POSITION PREMOVE THICK PORDER $ positioning blank on top of lower binder 1 3 3 1 0.7 blankmv $ positioning upper die on top of blank 2 3 1 1 0.7 updiemv $---+----1----+----2----+----3----+----4----+----5----+----6----+----7----+----8 *PARAMETER_EXPRESSION $ PRMR1 EXPRESSION R clstime (abs(updiemv)-vcls*tclsup)/vcls+2.0*tclsup R endtime &clstime $---+----1----+----2----+----3----+----4----+----5----+----6----+----7----+----8 *PART_MOVE $ PID XMOV YMOV ZMOV CID 1 0.0 0.0 &blankmv 2 0.0 0.0 &updiemv $---+----1----+----2----+----3----+----4----+----5----+----6----+----7----+----8 *CONTROL_TERMINATION &endtime Revision information: This feature is available starting in LS-DYNA Revision 56080 in both explicit and implicit, SMP and MPP versions. Later revisions are also available with various improvements. *CONTROL_FORMING_BESTFIT Available options include: <BLANK> VECTOR Purpose: This keyword rigidly moves a part to the target so that they maximally coincide. This feature can be used in sheet metal forming to translate and rotate a spring back part (source) to a scanned part (target) to assess spring back prediction accuracy. This keyword applies to shell elements only. The VECTOR option allows vector components of the normal distance from the target to the part node to be included keyword under *NODE_TO_TARGET_VECTOR . bestfit.out output the the file in This feature is available now in LS-PrePost 4.3 in Metal Forming Application/eZ Setup (http://ftp.lstc.com/anonymous/outgoing/lsprepost/4.3/win64/). Card 1 1 2 3 4 5 6 7 8 Variable IFIT NSKIP GAPONLY IFAST IFSET NSETS NSETT Type Default I 0 I -3 Card 2 1 2 I 0 3 Variable Type Default I 1 4 I 0 5 FILENAME A80 none I I none none 6 7 8 VARIABLE DESCRIPTION IFIT Best fit program activation flag: IFIT.EQ.0: do not perform best-fit. IFIT.EQ.1: activate the best-fit program. VARIABLE NSKIP DESCRIPTION Optional skipping scheme during bucket searching to aid the computational speed (zero is no skipping): NSKIP.GT.0: Number of nodes to skip in bucket searching. NSKIP of “1” does not skip any nodes in search- ing therefore computing speed is the slowest but accuracy is the highest. Higher values of NSKIP speed up the calculation time with slightly dete- riorating accuracies. Based on studies, a value of “5” is recommended with IFAST = 1, which bal- ances the speed and accuracy. See Table 12-21 for the effect of NSKIP on the accuracy of the fitting. NSKIP.LT.0: Absolute value is the distance to skip in bucket searching. This scheme is faster compared to the previous method and therefore is recommended for computational efficiency and accuracy. A value of “-5” is suggested. See Example 3. IFAST = 0 IFAST = 1 NSKIP CPU time 2 5 10 20 50 10 min 38 sec 4 min 49 sec 2 min 46 sec 1 min 24 sec 50 sec Max/Min (mm) 1.28/-1.59 1.21/-1.59 1.27/-1.59 1.27/-1.59 1.22/-1.61 CPU time 4 min 3 sec 1 min 59 sec 1 min 18 sec 59 sec 40 sec Max/Min (mm) 1.22/-1.59 1.25/-1.61 1.44/-1.53 1.42/-1.64 1.43/-1.67 Table 12-21. Computing speed and the max/min deviations from the springback mesh to the target scan for an automotive part, under various combinations of NSKIP and IFAST. All runs were made on a 1 CPU XEON E5520 machine, with 685132 elements on the target scan and 135635 elements on the springback mesh. VARIABLE DESCRIPTION GAPONLY Separation distance calculation flag: GAPONLY.EQ.0: perform best-fit, separation distances between the two best-fitted mesh parts. calculate GAPONLY.EQ.1: no best-fit, just calculate separation distances between the two existing mesh parts. GAPONLY.EQ.2: User is responsible to move the parts closer in distance and orientation, in situation where target and source are not similar in shape. Also see NSETS and NSETT (recommended method). IFAST Computing performance optimization flag: IFSET IFAST.EQ.0: no computing speed optimization. IFAST.EQ.1: activate computing speed optimization (default), and is recommended. See Table 12-21 for detailed speed performance data. Optional flag to define a node set to be included or excluded in the source mesh file for best fitting. The node set can be defined in a file together with the source mesh. A node set can be defined using LS-PrePost via menu options Model→CreEnt→Set Data→*SET_NODE→Cre. IFSET.EQ.0: all nodes in the source mesh file will be best fitted. IFSET.GT.0: the input value is a node set ID; only the nodes in VARIABLE DESCRIPTION the set will be best fitted. IFSET.LT.0: the absolute value is a node set ID; all nodes excluding those in the set will be best fitted. See Example 2. An optional node set ID of three nodes from the source mesh. The nodes should be selected based on distinctive geometry features, such as, the center of an arc, the center of a dart, or the end node of a take-up bead . The three nodes must not be aligned in one straight line. Define NSETS if the orientation of the source mesh deviates from the target is large (>~30 degrees in any direction). This is the recommended method. An optional node set ID from the target mesh, consists of the corresponding three nodes from the same geometry features of the source mesh. The three nodes should be input in the same order as those from the source mesh. Approximate locations are acceptable. Define NSETT only if NSETS is defined. See Example 3 and Figure 12-22 for details. This is the recommended method. Target mesh file in keyword format, where only *NODE and *EL- EMENT_SHELL should be included. The target mesh is typically the scanned part converted from the STL format file. STL file format can be imported into LS-PrePost via File→Import→STL File, then a keyword format mesh file can be saved. NSETS NSETT FILENAME Remarks: In springback prediction and compensation process simulation, there is always a need to assess the accuracy of the springback prediction using physical white-light scanned parts. Scanned parts are typically given in the STL format, which can be imported into LS-PrePost and written back out as a keyword mesh file. The converted scanned keyword file can be used as FILENAME as a target mesh in an input file . The predicted springback mesh (source), consisting of *NODE, *ELEMENT_SHELL, *CONSTRAIN_ADAPTIVITY cards only, can be included in the input file using *INCLUDE. The best-fit program uses an iterative least-squares method to minimize the separation distances between the two parts, eventually transforming the springback mesh (source) into the position of the target mesh (scan). The normal distances between the two parts are calculated after the best-fitting, and stored as thickness values in a file bestfit.out, which is essentially a dynain file. Both positive and negative distances are calculated and stored as the Thickness. Color contours of the normal distances between the two parts can then be plotted using COMP→Thickness. Positive distance means the source mesh is above the target mesh in a larger coordinates, and negative distance is below the target mesh in a smaller coordinates. For areas where no corresponding meshes can be found between the two parts, the distances are set to nearly zero. The fitting accuracy is within 0.02mm. To reduce the computing time , the scan file (STL) mesh can be coarsened in a scan- processing software from a typically very dense mesh to a more reasonably sized mesh. In any case, the coarser mesh should be selected as the target mesh for optimal computational speed. The fitted mesh bestfit.out and target mesh parts can both be imported into LS-PrePost. Using the SPLANE feature in LS-PrePost, multiple sections can be cut on both parts to assess springback deviations on a cut-section basis. It is suggested that the orientation of the included file (source) should be within 30 degrees in any direction of the target file. In addition, the more rotations needed to re- orient the include file to align with the target file, the more CPU time will it take to complete the best fitting. In case the source mesh orients more than 30 degrees in any directions of the target mesh, NSETS and NSETT can be used to initially align the source mesh to the target mesh before a full best-fit is performed. See Example 3 and Figure 12-22. Example 1 – fitting with all nodes from the included file: A complete input example is provided below to best fit a source mesh part spbk_ NoSS.k to the target mesh part scan.k. NSKIP is set to “-5” and speed optimization is activated by setting IFAST to “1”. *KEYWORD *CONTROL_FORMING_BESTFIT $ IFIT NSKIP GAPONLY IFAST IFSET 1 -5 0 1 0 scan.k *INCLUDE spbk_NoSS.k *END Example 2 – fitting with an excluded node set: From the previous example, the included source file spbk_NoSS.k now consists of node set 128. The node set, which is defined in the file spbk_NoSS.k, which may feature geometry that are not a part of the target mesh, is being excluded (IFSET = -128) from participating in the best fitting. Alternatively, the unwanted nodes can be just deleted from the source file. *KEYWORD *CONTROL_FORMING_BESTFIT $ IFIT NSKIP GAPONLY IFAST IFSET 1 -5 0 1 -128 scan.k *INCLUDE spbk_NoSS.k *END Example 3 – fitting with NSETS and NSETT (recommended): In the following partial keyword example (shown in Figure 12-22) a source mesh sourcemesh.k is being best fitted to a target mesh targetmesh.k. A node set with ID 1 on the source mesh is defined consisting of nodes 1001 1002 and 1003 and a corresponding node set with ID 2 on the target mesh is defined and consists of nodes 1, 2 and 3. Node ID 1001 and 1 are both located at the center of a dart on the top surface of the hat- shaped part. Node ID 1002 and 2 are selected at the center of an arc of an cutout hole. Lastly, node ID 1003 and 3 are at the center of a tangent line of a radius. With the NSKIP set a “-5”, the search will be done skipping every 5 mm of distance. In this example, since the source and target meshes are exactly the same, the normal distance, as displayed by “thickness” is nearly zero everywhere. *CONTROL_FORMING_BESTFIT $---+----1----+----2----+----3----+----4----+----5----+----6----+----7----+----8 $# IFIT NSKIP GAPONLY IFAST IFSET NSETS NSETT 1 -5 0 1 0 1 2 $# FILENAME targetmesh.k *INCLUDE sourcemesh.k *SET_NODE_LIST 1 1,2,3 *SET_NODE_LIST 2 1001,1002,1003 Revision information: This feature is available starting from LS-DYNA Revision 96427 double precision SMP. The variable IFSET is available starting from Revision 96696. The variables NSETS, NSETT are available starting from Revision 99369. The VECTOR option is available starting from Revision 112655. Node 1 Node 3 Node 1002 Node 2 Node 1001 Node 1003 Source mesh Target mesh Best fit results of part separation Contours of shell thickness min=-9.39123e-06 at elem# 102 max=8.45032e-06 at elem# 149 Node 1: geometry feature such as the center of a dart is a preferred choice to be one of the three nodes. Node 3: the center node of a tangent line may also be used. Node 2: the center of an arc of a hole can also be used to select one of the three nodes. Part Separation (mm) 8.450e-06 6.665e-06 4.881e-06 3.097e-06 1.313e-06 4.706e-07 -2.255e-06 -4.039e-06 -5.823e-06 -7.607e-06 -9.391e-06 Best fit results - color contour of part separation plotted with "thickness" from the output file "Bestfit.out" Figure 12-22. Best fit of two meshes with orientations greater than 30 degrees from each other. *CONTROL_FORMING_INITIAL_THICKNESS Purpose: This keyword is used to specify a varying thickness field in a specific direction on a sheet blank (shell elements only) as a result of a metal forming process such as a tailor-rolling, to be used for additional metal forming simulation. Another related keyword includes *ELEMENT_SHELL_THICKNESS. Card 1 1 2 Variable PID LCID Type I I 3 X0 F 4 Y0 F 5 Z0 F/I 6 VX F 7 VY F 8 VZ F Default none none none none none none none none VARIABLE DESCRIPTION PID LCID Part ID of the sheet blank to be defined with varying thickness, as in *PART. Currently only 1 PID is allowed. Load curve ID defining thickness (Y-values) vs. distance (X- values) starting from position coordinates (X0, Y0, Z0) and in the direction of a vector [VX, VY, VZ], as in *DEFINE_CURVE. X0, Y0, Z0 Starting position coordinates. VX, VY, VZ Vector components defining the direction of the distance in the load curve. Background: Tailor-rolling is a process used to vary the thickness of the blank. A judiciously designed and manufactured tailor-rolled blank will reduce the number of parts (reinforcements) involved in the stamping process, as well as the number tools needed to make them. By reducing the number of spot welds, tailor-rolled pieces also possess superior structural integrity. Remarks: 1. Beyond the last data point LS-DYNA extrapolates the load curve specified in LCID as being constant. 2. This card overrides thicknesses set with the *SECTION_SHELL keyword. Application example: An excerpt from an input deck containing a characteristic example of this card’s application is given below. In this example the blank is part ID 1. The axis of the load curve starts at position (−295, −607, −43) and the direction along which the load curve sets the thickness is given by (524, 607, 0). For each of the load curve’s abscissa values, 𝑡, the corresponding geometrical coordinate is given by: 𝒓 = −295 −607 −43 ⎦ ⎥⎤ + ⎢⎡ ⎣ 524 607 0 ⎦ ⎥⎤ 𝑡 ⎢⎡ ⎣ For negative values along the load curve, 𝑡 < 0, and values of 𝑡 > 101.0, the thickness is extrapolated as a constant value of 0.8, and 0.9, respectively. *CONTROL_FORMING_INITIAL_THICKNESS $ PID LCID X0 Y0 Z0 VX VY VZ 1 1012 -295.0 -607.0 -43.0 524.0 607.0 0.0 *DEFINE_CURVE 1012 0.0, 0.8 21.0, 0.9 43.0, 1.0 65.0, 1.1 82.0, 1.0 101.0, 0.9 In Figure 12-23, a sheet blank is defined with a varying thickness across its surface in a vector direction pointed from the start to end point. The thickness variation vs. the distance from starting point in section A-A is shown in Figure 12-24. Revision information: This feature is available in LS-DYNA starting in Revision 82990. Contours of shell thickness min=0.635661 at elem# 175119 max=1.29457 at elem# 177147 Ending point (distance=802mm) Starting point (distance=0) Thickness (mm) 1.295 1.229 1.163 1.097 1.031 0.965 0.899 0.833 0.767 0.702 0.636 Figure 12-23. Define a varying thickness field across the sheet blank. Input Response ) ( 1.4 1.3 1.2 1.1 1.0 0.9 0.8 0.7 0.6 0.0 200.0 400.0 600.0 800.0 Distance Along Section (mm) Figure 12-24. Thickness variation across section A-A *CONTROL_FORMING_MAXID Purpose: This card sets the node and element ID numbers for an adaptive sheet blank. The new node and element number of the adaptive mesh will start at the values specified on this card, typically greater than the last node and element number of all tools and blanks in the model. This keyword is often used in multi-stage sheet metal forming simulation. The *INCLUDE_AUTO_OFFSET keyword is related. Card 1 1 2 3 4 5 6 7 8 Variable PID MAXIDN MAXIDE Type I I I Default none none none VARIABLE DESCRIPTION PID Part ID of the sheet blank, as in *PART. Node ID number from which adaptive node ID numbers will be created. Element ID number from which adaptive element ID numbers will be created. MAXIDN MAXIDE Remarks: In a multi-stage automatic line die simulation the adaptivity feature may generate node and element IDs that collide with those of the tools used in the later stages of the process. Before the calculation begins, the set of IDs used by the tools is known. By setting MAXIDN to a value greater than the largest tool node ID and MAXIDE to a value greater than the largest tool element ID, it is guaranteed that refinement during the early stages will not lead to conflicts with tool IDs in the later stages. The following example shows this feature applied in a 2D trimming simulation. Nodes and elements ID numbers generated from an adaptive trim simulation will be larger than the specified ID numbers of 5921980 and 8790292, respectively, for a sheet blank with part ID of 4. *KEYWORD *INCLUDE_TRIM sim_trimming.dynain ⋮ *CONTROL_ADAPTIVE_CURVE $ IDSET ITYPE N SMIN &blksid 2 2 0.6 *CONTROL_CHECK_SHELL $ PSID IFAUTO CONVEX ADPT ARATIO ANGLE SMIN &blksid1 1 1 1 0.250000150.000000 0.000000 *INCLUDE EZtrim.k $---+----1----+----2----+----3----+----4----+----5----+----6----+----7----+----8 *DEFINE_CURVE_TRIM_NEW $# tcid tctype tflg tdir tctol toln nseed1 nseed2 90914 2 0 1 1.250000 1.000000 0 0 sim_trimming_trimline_01.igs *DEFINE_VECTOR $# vid xt yt zt xh yh zh cid 1 0.000 0.000 0.000 0.000 0.000 1.000000 0 *CONTROL_FORMING_MAXID $ pid maxidn maxide 4 5921980 8790292 *END Revision Information: This feature is available starting in LS-DYNA Revision 84159. *CONTROL_FORMING_ONESTEP_{OPTION} Purpose: This keyword activates a one-step solution using the total strain theory approximation to plasticity (also known as deformation theory) to implement an inverse method. Given the final geometry, the one-step method uses LS-DYNA’s implicit statics solver to compute an approximate solution for (1) the stresses and strains in the formed part, (2) the thickness of the formed part, and (3) the size of the initial blank (unfolded flat blank). This method is useful for estimating the initial blank size with attendant material costs, and for augmenting crashworthiness models to account for metal forming effects, such as plastic strains and blank thickness in crash simulation. NOTE: The input must contain only one “part”, consisting entirely of shells, which is taken to be the final geometry. 1. This “part” may involve more than one PID to accommo- date welded blanks, 2. 3. it must be composed entirely of shells, and, its external boundary must consist of a single closed loop. Keywords associated with *CONTROL_FORMING_ONESTEP are: *CONTROL_FORMING_UNFLANGING *INTERFACE_BLANKSIZE_DEVELOPMENT. Available options include: <BLANK> AUTO_CONSTRAINT DRAWBEAD FRICTION TRIA QUAD QUAD2 (default) Summary of keyword options: 1. The AUTO_CONSTRAINT option excludes rigid body motion from the implicit solution by automatically adding nodal constraints. A deck with a *CON- TROL_FORMING_ONESTEP card should contain at most one *CONTROL_- FORMING_ONESTEP_AUTO_CONSTRIANT card. In addition, starting from Revision 91229, three nodes can be specified on the final part to position the unfolded blank for easier blank nesting, and for blank alignment in forming simulation. 2. The DRAWBEAD option is used to apply draw bead forces in addition to those provided by AUTOBD field in Card 1. A deck containing a *CONTROL_- FORMING_ONESTEP card may contain as many *CONTROL_FORMING_ON- ESTEP_DRAWBEAD cards as there are draw beads to be defined. 3. The FRICTION option applies friction along the edge of the part based on the binder tonnage input by the user in the DBTON field of card 1. A deck contain- ing a *CONTROL_FORMING_ONESTEP card may contain as many *CON- TROL_FORMING_ONESTEP_FRICTION cards as there are friction node sets to be defined. 4. Originally all quadrilateral elements in the model were split into two triangular elements internally for calculation. This original formulation is set as option TRIA as of Revision 112682. The option QUAD supports quadrilateral elements and implements some improved algorithm, which result in better results. In addition, this option greatly improves calculation speed under multiple CPUs in SMP mode, and is available starting in Revision 112071. The option QUAD2 is yet another improvement over the option QUAD with enhanced element formulation, which further improves results in terms of thinning and plastic strain with slightly longer CPU times. Calculation speed comparisons among the three options can be found in Performance among options TRIA, QUAD. The option QUAD2 is set as a default as of Revision 112682 and is the recom- mended option. Card 1 for no option, <BLANK>. Card 1 1 2 3 4 5 6 7 8 Variable OPTION TSCLMAX AUTOBD TSCLMIN EPSMAX LCSDG DMGEXP Type Default I 6 F F F F I F 1.0 0.0 1.0 1.0 none none Card 1 for option AUTO_CONSTRAINT. Card 1 1 2 3 4 5 6 7 8 Variable ICON NODE1 NODE2 NODE3 Type I I I I Default none none none none Card 1 for option DRAWBEAD. Card 1 1 2 3 4 5 6 7 8 Variable NDSET LCID TH PERCNT Type I I F F Default none none 0.0 0.0 Card 1 for option FRICTION. Card 1 1 2 3 4 5 6 7 8 Variable NDSET BDTON FRICT Type I F F Default none 0.0 0.12 Card 2 for no option <BLANK>. Card 2 1 2 3 4 5 6 7 8 Variable Type Default VARIABLE OPTION TSCLMAX FLATNAME A none DESCRIPTION Options to invoke the one-step solution methods which account for undercut conditions in the formed part: EQ.6: One-step solution with unfolded blank (flat) provided by LS-PrePost . Card #2 is required. EQ.7: One-step solution with blank automatically unfolded in LS-DYNA. Card #2 is a blank line. This option is rec- ommended. L.T.0: If a negative sign precedes any of the above OPTIONs, the stress and strain output in the file onestepresult will be in a large format (E20.0), which leads to more accurate stress results. If not zero, it defines a thickness scale factor limiting the maximum thickness in the part. For example, if the maximum thickness allowed is 0.8mm for a blank with initial thickness of 0.75mm TSCLMAX can be set to 1.0667. All thicknesses that are computed as more than 0.8mm in the sheet blank will be reset to 0.8mm. The scale factor is useful in advance feasibility analysis where part design and stamping process have not been finalized and could potentially cause large splits or severe wrinkles during unfolding, rendering the forming results unusable for crash/safety simulation. AUTOBD TSCLMIN EPSMAX LCSDG DMGEXP *CONTROL_FORMING_ONESTEP DESCRIPTION Apply a fraction of a fully locked bead force along the entire periphery of the blank. The fully locked bead force is automatically calculated based on a material hardening curve input. AUTOBD can be increased to easily introduce more thinning and effective plastic strain in the part. LT.0.0: Turns off the “auto-bead” feature. EQ.0.0: Automatically applies 30% of fully locked force. GT.0.0: Fraction input will be used to scale the fully locked force. If not zero, it defines a thickness scale factor limiting the maximum thickness reduction. For example, if the minimum thickness allowed is 0.6mm for a blank with initial thickness of 0.75mm TSCLMIN can be set to 0.8. All thicknesses that are computed as less than 0.6mm in the sheet blank will be reset to 0.6mm. The scale factor is useful in advance feasibility analysis where part design and stamping process have not been finalized and could potentially cause large splits or severe wrinkles during unfolding, rendering the forming results unusable for crash/safety simulation. If not zero, it defines the maximum effective plastic strain allowed. All computed effective plastic strains that are greater than this value in the blank will be set to this value. Load curve ID defining equivalent plastic strain to failure vs. stress triaxiality, see *MAT_ADD_EROSION. for see Exponent *MAT_ADD_EROSION. Damage accumulation is written as history variable #6 in the file onestepresult. accumulation, nonlinear damage ICON Automatic nodal constraining option to eliminate the rigid body motion: EQ.1: Apply. VARIABLE NODE[1,2,3] NDSET LCID TH DESCRIPTION Node IDs for which the position is fixed during the unfolding. The position of these nodes in the calculated unfolded piece will coincide with the corresponding nodes in the input. The transformed and unfolded blank will be written in a keyword file “repositioned.k”. When these fields are undefined the orientation of the unfolded blank is arbitrary. Node set ID along the periphery of the part, as defined by keyword *SET_NODE_LIST. Load curve ID that defines the material hardening curve. Thickness of the unformed sheet blank. PERCNT Draw bead lock force fraction of the fully locked bead force. BDTON Binder tonnage used to calculate friction force. FRICT Coefficient of friction. FLATNAME File name of the initial unfolded blank by LS-PrePost . This is needed only for the OPTION = 6. Leave a blank line for OPTION = 7. About One-Step forming solution: One-step solution employs the total strain (or deformation) theory of plasticity in place of the more realistic incremental strain (or flow) theory. The total deformation theory expresses stress as a function of total strain; whereas the incremental strain theory requires that LS-DYNA compute a stress update at each time step (strain increment) from the deformation that occurred during that time step. In deformation theory, the results, therefore, do not depend on strain path, forming history, or the details of the stamping process. When this card is included, the input must contain the final geometry from which LS- DYNA calculates the initial flat state using the inverse method. The one-step solution results can get close to the incremental results only when the forming process involves a linear strain path for which the deformation is either monotonically increasing or decreasing. In most cases total strain theory does not match incremental forming. Path independence leads to several key simplifications: 1. Binder and addendum geometry are not required. There is no need to measure or model these geometries. 2. The solution is independent of stamping die processes (including part tipping). 3. There is no need for contact treatment since there are no tools and dies involved. The one-step solution is mostly used for advance formability studies in which the user needs to quickly compare a wide range of different design alternatives. With this method the user can evaluate blank size, estimate material cost, and generate a first guess for blank size development . This method is also widely used to initialize forming stresses and strains in crash and occupant safety analysis. Input details: 1. Mesh. In addition to the usual material and physical property definitions, this method requires that the final part be fully meshed using shell elements. This mesh must satisfy a different set of requirements than the tooling mesh. In particular, along the part bend radius, there is no need to build six elements along the arc length as one would do for the punch/die radius; two elements may be enough. A mesh consisting of uniformly distributed quadrilateral shell elements is ideal. All elements in the mesh must also have normal consistency. With LS-PrePost 4.0, this kind of mesh can be generated using Mesh → AutoM → Size. Since this method uses an implicit static solution scheme, the computa- tional cost is controlled by the number of elements; element size has no effect. Furthermore, it is important to note that if one wants to obtain forming results that are closer to the incremental forming results, the part in the one-step input should be similar in size to the final formed blank shape in the incremental forming (before trimming). 2. Holes. Any trimmed-out holes can be filled (but not necessary). The filling can be done semi-automatically using LS-PrePost 4.0 by selecting Mesh → EleGen → Shell → Shell by Fill_Holes → Auto Fill. The filled area of the part can be saved in a different part, as multiple parts (PID) are allowed. The forming results may depend on whether or not the holes are filled. 3. Unfolding. For OPTION = 6, the unfolded blank can be obtained from LS- PrePost via EleTol → Morph → Type = Mesh_Unfolding → Unfold. The unfolded mesh can be saved as a keyword file and used as input . With OPTION = 7, LS-DYNA unfolds the mesh itself. 4. Element Formulation. Shell element of type 2 and 16 are supported. Since this feature uses the implicit method, type 16 is more convergent, computationally efficient, and, therefore, strongly recommended. Results are output on all inte- gration points, as seen in the ELFORM and NIP variables in *SECTION_SHELL. 5. Supported Materials. Currently, *MAT_024, and *MAT_037 are supported. The user must provide a material hardening curve either in the LCSS field of *MAT_024 or in the HLCID field of *MAT_037. For *MAT_024 tables are sup- ported. Future releases will add support for bilinear hardening with the ETAN feature. Additionally, in *MAT_024, strain rate is ignored, even when the vari- ables C, and P are set. 6. Boundary Conditions. The primary “boundary/loading condition” for the one-step solution is the draw bead forces, which are set with the AUTOBD field or with the DRAWBEAD keyword option. a) With the DRAWBEAD option, draw bead forces are applied on a user de- fined node set . A fraction of the full lock force, determined by the tensile strength and sheet thickness, can be specified. The larger the fraction, the less the metal will flow into the die resulting in more stretching and thinning. b) Boundary conditions may also be set using the “Auto Beads” feature with which draw bead forces are automatically ap- plied to all nodes along the part boundary. The users must specify the fraction of the fully locked bead force to be applied. The default value of 30% is sufficient for crash/occupant safety applications. The last important, but often overlooked, “boundary condition” is the part’s shape. For example, an oil pan with a larger flange area will experience greater thinning in the part wall, whereas having a smaller flange area will have the reverse effect. To obtain results that are closer to the incremental strain theory, additional materials may need to be added to the final part geometry in cases where the sheet blank is not “fully developed,” meaning no trimming is re- quired to finish the part. 7. Friction. Friction effects can be included with the FRICTION option. The frictional force is based on an expected binder tonnage, and is a percentage of the input force. Note that the binder tonnage value is used exclu- sively in calculating friction forces. The binder tonnage is not actually applied on the binder as a boundary condition. 8. Rigid Body Motion. LS-DYNA will automatically add nodal constraints to prevent rigid body motion when the AUTO_CONSTRAINT option is used and ICON is set to 1. 9. Implicit Solver Options. All other implicit cards, such as *CONTROL_IM- *CONTROL_IM- PLICIT_GENERAL, PLICIT_SOLVER, *CONTROL_IMPLICIT_- TERMINATION, etc., are used to set the convergence tolerance, termination criterion, etc. The two most important variables controlling the solution con- *CONTROL_IMPLICIT_SOLUTION, *CONTROL_IMPLICIT_AUTO, vergence are DELTAU from *CONTROL_IMPLICIT_TERMINATION, and DCTOL from *CONTROL_IMPLICIT_SOULTION. Experience has shown that they should be set to 0.001 and 0.01, respectively, to obtain the most efficient solution with the best results. Typically, four implicit steps are sufficient, and DT0 in *CONTROL_IMPLICIT_GENERAL and ENDTIM in *CONTROL_TER- MINATION should be set accordingly. For difficult parts, more steps maybe needed. For some parts, ILIMIT in *CONTROL_IMPLICIT_SOLUTION may need to be set to “1” for the full Newton iteration. 10. Blank Card. Card #2 for no option <BLANK> is a blank card, but it must be present. Output: Results are stored in an ASCII file named “onestepresult” using the dynain format. This file contains the forming thickness, the stress and the strain fields on the final part. It can be plotted with LS-PrePost. One quick and useful LS-PrePost plotting feature is the “formability contour map”, which colors the model to highlight various forming characteristics including cracks, severe thinning, wrinkles, and good surfaces. The formability map feature is located in Post → FLD → Formability. Additionally, the final estimated blank size in its initial, flat state is stored in the d3plot files. The d3plot files also contain intermediate shapes from each implicit step. The final blank mesh in its flat state can be written to a keyword file using LS-PrePost by the following steps: 1. Go to Post → Output → Keyword, 2. check the box to include Element and Nodal Coordinates 3. move the animation bar to the last state, and, 4. click on Curr and Write. In addition, blank outlines can be created by: 1. menu option Curve → Spline → From Mesh (Method), 2. 3. 4. 5. checking Piecewise → byPart, select the blank, click on Apply, and, finally, save the curves in IGES format using the File menu at the upper left corner. Effect of TSCLMAX, TSCLMIN and EPSMAX: During the early stage of product design, the initial product specifications may lead to large strains and excessive thinning on the formed panel. The ensuing one-step results would not be suitable to be used in a crashworthiness simulation. However, these kinds of forming issues are certain to be fixed as a natural part of the design and stamping engineering process. The variables TSCLMAX, TSCLMIN and EPSMAX are thus created to impose artificial limits on the thinning and plastic strains. The variables provide convenient way to run a crash simulation with approximate and reasonable forming effects before the design is finalized. In the keyword below (which is a part of the firewall model with original thickness of 0.75mm), TSCLMIN and EPSMAX are set to 0.8 and 0.3, respectively. *CONTROL_FORMING_ONESTEP $ OPTION TSCLMAX AUTODB TSCLMIN EPSMAX 7 0.5 0.8 0.3 The thickness and effective plastic strain plots for the firewall model are shown in Figures 12-29 and 12-30, respectively. The minimum value in the thickness contour plot and maximum value in the plastic strain contour plot as shown in the upper left corner correspond to the values specified in TSCLMIN and EPSMAX, respectively. Similarly, TSCLMAX can be set to 1.0667 to limit the max thickening in the part to 0.8mm: *CONTROL_FORMING_ONESTEP $ OPTION TSCLMAX AUTODB TSCLMIN EPSMAX 7 1.0667 0.5 0.8 0.3 Reposition of unfolded flat blank: Often times the input to one-step simulation is the final product part in the car axis system. However, after the simulation, the unfolded flat blank will be in a different orientation and position, requiring users to manually reposition the blank to its desired orientation and position. The variables NODE1, NODE2, NODE3 allow users to specify three nodes so that the blank is transformed onto the final part (the input), superimposing the exact same three nodes in both parts. In an example shown in Figure 12-32, the three nodes (Nodes 197, 210 and 171) are defined near the edges of two holes. The transformed and unfolded flat blank (written in a keyword file “reposi- tioned.k”) is seen superimposed onto the final part according to the three nodes specified (Figure 12-32 bottom). If these nodes are not defined, the simulation will result in the unfolded flat blank in a state shown in Figure 12-32 (top), undesirable to most users. Damage accumulation D *MAT_ADD_EROSION): *CONTROL_FORMING_ONESTEP is calculated based on (refer to manual section DMGEXP 𝐷 = ( 𝜀𝑝 𝜀𝑓 ) In the example below, load curve #500 provides plastic failure strain vs. stress triaxiality and DMGEXP is assumed to be 1.254. Since the damage accumulation is written into the file onestepresult as history variable #6, the variable NEIP in *DATABASE_EXTENT_BINARY should be set to at least ‘6”. *CONTROL_FORMING_ONESTEP $ OPTION AUTODB TSCLMIN EPSMAX LCSDG DMGEXP 7 0.8 0.3 500 1.254 *DEFINE_CURVE 500 -0.3,0.6 -0.2,0.3 0.0,0.2 0.2,0.25 0.4,0.46 0.65,0.28 0.9,0.18 *DATABASE_EXTENT_BINARY $ NEIPH NEIPS MAXINT STRFLG SIGFLG EPSFLG RLTFLG ENGFLG 6 7 1 $ CMPFLG IEVERP BEAMIP DCOMP SHGE STSSZ 1 2 The damage accumulation contour map from the file onestepresult can be plotted in LS- PrePost. Effect of hole-cut on the forming results: In Figure 12-31, a thickness contour plot of a one-step calculation on the NCAC Taurus firewall model with its holes unfilled is shown. The unfilled case will undergo slightly less thinning, since the holes will expand as material flows outward away from the hole. However, the thicknesses with holes filled are likely closer to reality, since the holes are mostly filled during forming on the draw panel and then trimmed off afterwards in a trim process. On the other hand, it is important to realize that not all the holes are filled in a draw panel. Some holes are cut inside the part in the scrap area (but not all the way to the trim line) during draw process to allow material to flow into areas that are difficult to form, so as to avoid splitting. Application example: The following example provides a partial input file with typical control cards. It will iterate for four steps, with auto beads of 0% lock force applied around the part boundary, and with automatic nodal constraints. *CONTROL_TERMINATION $ ENDTIM 1.0 *CONTROL_IMPLICIT_GENERAL $ IMFLAG DT0 1 0.25 *CONTROL_FORMING_ONESTEP $ OPTION AUTODB 7 *CONTROL_FORMING_ONESTEP_AUTO_CONSTRAINT $ ICON 1 *CONTROL_IMPLICIT_TERMINATION $ DELTAU 0.001 *CONTROL_IMPLICIT_SOLUTION $ NSLOLVR ILIMIT MAXREF DCTOL ECTOL 2 11 1200 0.01 1.00 *CONTROL_IMPLICIT_SOLVER $ LSOLVR 5 *CONTROL_IMPLICIT_AUTO $ IAUTO ITEOPT ITEWIN DTMIN DTMAX 0 0 0 0.0 0.0 Additional cards below specify extra bead forces of 45% and 30% applied to node sets 22 and 23 along the part periphery, respectively. Also, the resulting friction forces with friction coefficient of 0.1 and binder tonnage of 10000.0 N used for friction force are applied on the same node sets. *CONTROL_FORMING_ONESTEP_DRAWBEAD $ NDSET LCID TH PERCNT 22 200 1.6 0.45 *CONTROL_FORMING_ONESTEP_DRAWBEAD 23 200 1.6 0.30 *CONTROL_FORMING_ONESTEP_FRICTION $ NDSET BDTON FRICT 22 10000.0 0.1 *CONTROL_FORMING_ONESTEP_FRICTION $ NDSET BDTON FRICT 23 10000.0 0.1 The one-step forming results for the NCAC Taurus model’s firewall are shown in Figure 12-25. The average element size across the blank is 8mm, and the trimmed part (with holes filled) consists of 15490 elements. *MAT_24 was used with BH210 material properties. On a 1 CPU Xeon E5520 Linux machine, it took 4 minutes to complete the run with a total of four steps. The thickness, the plastic strain, and the blank size prediction were reasonable, as shown in Figures 12-26, 12-27 and 12-28. Performance among options TRIA, QUAD and QUAD2: The following partial keyword input is an example of using the option QUAD. Note the draw bead force parameter AUTOBD is set at 0.5. Calculation speed comparison among options QUAD, QUAD2 and TRIA can be found in Table 12-1. *KEYWORD *include model.k *CONTROL_TERMINATION 1.0 *CONTROL_FORMING_ONESTEP_QUAD $# option maxthick autobd thinmin epsmax 7 0.5 *CONTROL_FORMING_ONESTEP_AUTO_CONSTRAINT 1 *CONTROL_IMPLICIT_GENERAL $# imflag dt0 imform nsbs igs cnstn form zero_v 1 0.2500 2 1 0 0 0 0 *CONTROL_IMPLICIT_TERMINATION $# deltau delta1 ketol ietol tetol nstep 0.001000 0.000 0.000 0.000 0.000 0 *CONTROL_IMPLICIT_NONLINEAR $# nsolvr ilimit maxref dctol ectol not used lstol rssf 12 11 200 0.010000 0.100000 0.000 0.000 0.000 $# dnorm diverg istif nlprint 0 0 0 2 $# arcctl arcdir arclen arcmth arcdmp 0 0 0.000 1 2 *CONTROL_IMPLICIT_SOLVER 5 *PART 5000000 5000000 5000000 *SECTION_SHELL 5000000 16 1. 5. 1. 0.72 0.72 0.72 0.72 ... Table 12-1 Calculation speed improvement with and without option _QUAD. Number of elements Calculation speed (D.P. SMP Rev.112720, 8 CPUs) Option TRIA Option QUAD Option QUAD2 A hat shape part 71000 21.0 min 14.1 min 16.6 min A upper dash panel 61700 24.5 min 11.5 min 17.2 min Revision information: This feature is available starting in Revision 67778 SMP and double precision only. Over time, improvements are made to improve accuracy and speed up the calculation time; revision 110117 or later is recommended. Historic revisions are listed as follows: 1)Revision 73442: output of stress tensors 2)Revision 75156: output of strain tensors. 3)Revision 75854: variables THINPCT and EPXMAX are available. 4)Revision 76709: holes are allowed. 5)Revision 91229: variables NODE1, NODE2, NODE3 are available. 6)Revision 108229: variables LCSDG and DMGEXP are available. 7)Revision 111311: variable TSCLMAX is available. 8)Revision 112071: option QUAD is available. 9)Revision 112682: original formulation is designated as option TRIA. A new option QUAD2 is activated. 10)Revision 109680: negative value of OPTION for a large format stress and strain output. Figure 12-25. A trimmed dash panel (firewall) with holes auto-filled using LS-PrePost 4.0 (original model courtesy of NCAC Taurus crash model). Contours of shell thickness min=0.478084, at elem# 3210698 max=1.10908, at elem# 3211511 Thickness (mm) 0.750 0.725 0.700 0.675 0.650 0.625 0.600 0.575 0.550 0.525 0.500 Figure 12-26. Shell thickness prediction (t0 = 0.75mm). Contours of plastic strain max ipt. value min=0, at elem# 3008783 max=0.46, at elem# 3210698 Plastic strain 0.460 0.414 0.368 0.322 0.276 0.230 0.184 0.138 0.092 0.046 0.000 Figure 12-27. Effective plastic strain Prediction. Figure 12-28. Initial blank size prediction (flat, not to scale). Contours of shell thickness min=0.6, at elem# 3206053 max=0.923214, at elem# 3211511 Thickness (mm) 0.750 0.725 0.700 0.675 0.650 0.625 0.600 0.575 0.550 0.525 0.500 Figure 12-29. Blank thickness prediction with TSCLMIN = 0.8. Contours of plastic strain max ipt. value min=0, at elem# 3008801 max=0.3, at elem# 3204379 Plastic strain 0.300 0.270 0.240 0.210 0.180 0.150 0.120 0.090 0.060 0.030 0.000 Figure 12-30. Effective plastic strain with EPSMAX = 0.3. Contours of shell thickness min=0.538193, at elem# 3209452 max=0.974493, at elem# 3211511 Thickness (mm) 0.750 0.725 0.700 0.675 0.650 0.625 0.600 0.575 0.550 0.525 0.500 Figure 12-31. Blank thickness with trimmed holes (t0 = 0.75mm). Unfolded flat blank Final part Final part Unfolded flat blank N197 Figure 12-32. An example of the results when using the NODE1, NODE2, and NODE3 feature (bottom) and without using the feature (top), courtesy of Kaizenet Technologies Pvt Ltd, India. N210 N171 *CONTROL_FORMING_OUTPUT_{OPTION} Available options include: <BLANK> INTFOR Purpose: This card defines the times at which states are written to the d3plot and intfor files based on the tooling’s distances from the home (final) position. When the INTFOR option is set this keyword card controls when states are written to the intfor file, otherwise it controls the d3plot file. This feature may be combined with parameterized input and/or automatic positioning of the stamping tools using the *CONTROL_- FORMING_AUTOPOSITION_PARAMETER card. NOTE: When this card is present no states are written except for those specified on this card. This card supersedes the *DATABASE_BINARY_D3PLOT card. Forming Output Cards. Repeat as many times as needed to define additional outputs in separate tooling kinematics curves. The next keyword (“*”) card terminates the input. Card 1 1 2 3 4 5 6 Variable CID NOUT TBEG TEND Y1/LCID Y2/CIDT 7 Y3 F 8 Y4 F Type I Default none I 0 F F F/I F/I 0.0 none none none none none VARIABLE CID DESCRIPTION ID of a tooling kinematics curve. This curve is integrated so that the specified output distances can be mapped to times. For correct distance-to-time mapping CID must be applied to the tool of interest using a *BOUNDARY_PRESCRIBED_MOTION_- RIGID card. The ordinate scale factor SFO in the *DEFINE_- CURVE is supported in this keyword starting from Revision 82755. ) ( - 0.0 -10 -20 -30 -40 -50 Y1 Y2 Y3 Y4 NOUT &clstime Punch displacement NOUT Y1 Y2 Y3 Y4 &endtime 0.0 0.002 0.004 0.006 0.008 0.01 0.012 Explicit time (sec.) Figure 12-33. An output example for closing and drawing. See the example provided at the end of this section. VARIABLE NOUT TBEG TEND DESCRIPTION Total number states written to the d3plot or intfor databases for the tooling kinematics curve, CID, excluding the beginning and final states. If NOUT is larger than the number of states specified by either LCID or Yi fields (5 through 8), the remaining states are evenly distributed between TBEG and the time corresponding to the biggest Yi from the home position, as shown in Figure 12-33. If NOUT is left as blank or as “0”, the total number of output states will be determined by either LCID or Yi’s. Start time of the curve. This time should be consistent with the BIRTH in *BOUNDARY_PRESCRIBED_MOTION_RIGID. End time of the curve. This time should be consistent with the DEATH in *BOUNDARY_PRESCRIBED_MOTION_RIGID. This time is automatically reset backward removing any idling time if the tool finishes traveling early, so output distances can start from the reset time. A state is written at TEND. Y1/LCID, Y2, Y3, Y4 Y2/CIDT *CONTROL_FORMING_OUTPUT DESCRIPTION Y1/LCID.GT.0: All four variables (Y1, Y2, Y3, Y4) are taken to be the distances from the punch home, where d3plot files will be output. Y1/LCID.LT.0: The absolute value of Y1/LCID (must be an integer) is taken as a load curve ID . Only the abscissas in the load curve, which are the distances to punch home, are used. These distances specify the states that are written to the d3plot files. Ordinates of the curve are ignored. This case accommodates more states than is possible with the four varia- Furthermore, when bles Y1, Y2, Y3, Y4. Y1/LCID < 0, Y2, Y3, and Y4 are ignored. Available starting from Revision 112604, the output will be skipped for any negative abscissa in the load curve. Note all abscissas being nega- tive are not allowed. Y2/CIDT.GT.0: The input is taken as the distance from the punch home, where a d3plot file will be output. Y2/CIDT.LT.0: The absolute value of Y2/CIDT (must be an integer) is taken as a load curve ID . Only the abscissas in the load curve, which are the simulation times, are used. These times specify the states that are written to the d3plot files. Ordinates of the curve are ig- nored. Note this time-dependent load curve will output additional d3plot files on top of the d3plot files already written in case Y1/LCID < 0 (if specified). Furthermore, when Y2/CIDT < 0, Y3 and Y4 are ignored. See an example for us- age. Motivation: In stamping simulations not all time steps are of equal interest to the analyst. This feature allows the user to save special states, usually those for which wrinkling and thinning conditions arise as the punch approaches its home position. This feature is available in Application eZ-Setup in LS-PrePost4.0 (http://ftp.lstc.com/- anonymous/outgoing/lsprepost/4.0/metalforming/). Remarks: 1. Keywords *DATABASE_BINARY_D3PLOT and *DATABASE_BINARY_INT- FOR are not required (ignored if present) to output D3PLOT and INTFOR files when this keyword is present; 2. 3. *CONTROL_FORMING_OUTPUT and *CONTROL_FORMING_OUTPUT_- INTFOR can share the same CIDs; If columns 5 through 8 are left blank, output (NOUT) will be evenly distributed through the travel; 4. The variable NOUT has priority over the number of points on the LCID; 5. Distances input (in LCID) that are greater than the actual tool travel will be ignored; 6. Distance input (in LCID) does not necessarily have to be in a descending or ascending order. Applicability: This keyword is applicable to the parameter VAD of “0” (velocity) in *BOUNDARY_- PRESCRIBED_MOTION_RIGID, and for explicit dynamics only. Tooling kinematics profiles of various trapezoids (including right trapezoid) are all supported. Local coordinate systems are supported. Y1 Y2 Y3 Y4 &vcls 0.0 &tramp &clstime Explicit time Figure 12-34. Specifying d3plot/intfor output at specific distances to punch home. Application example for an air draw: In a keyword example below (air draw, referring to Figures 12-33 and 12-35), a total of five states will be output during a binder closing. The kinematics are specified by the curve of ID 1113, which defines tooling kinematics starting time 0.0 and ending at time &clstime. Curve 1113 is used to associate the specified distances to the appropriate time step. In this example NOUT is set to 5. Of these five outputs states the last four will be output at upper die distance to closing of 3.0, 2.0, 1.0, and 0.5 mm according to the values specified in the Y1, Y2, Y3, and Y4 fields. Similarly, a total of eight states will be written to the d3plot file made during draw forming according curve ID 1115, which defines tooling kinematics starting at time &clstime, and ending at time &endtime. Of the eight states the last four will be output at punch distance to draw home of 6.0, 4.0, 3.0, and 1.0 mm; the remaining four outputs will be evenly distributed between starting punch distance to home and punch distance of 6.0mm to home. Likewise, for intfor, 15 states will be written before closing and 18 states after the closing. The d3plot and intfor files will always be output for the first and last states as a default; and at where the two curves meet at &clstime, only one d3plot and intfor will be output. To output intfor, “S=filename” needs to be specified on the command line, and SPR and MPR need to be set to “1” on the *CONTACT_… cards. $---+----1----+----2----+----3----+----4----+----5----+----6----+----7----+----8 *CONTROL_FORMING_OUTPUT $ CID NOUT TBEG TEND y1 y2 y3 y4 1113 5 &clstime 3.0 2.0 1.0 0.5 1115 8 &clstime &endtime 6.0 4.0 3.0 1.0 *CONTROL_FORMING_OUTPUT_INTFOR $ CID NOUT TBEG TEND y1 y2 y3 y4 1113 15 &clstime 3.5 2.1 1.3 0.7 1115 18 &clstime &endtime 16.0 4.4 2.1 1.3 *BOUNDARY_PRESCRIBED_MOTION_RIGID $ typeID DOF VAD LCID SF VID DEATH BIRTH &udiepid 3 0 1113 -1.0 0 &clstime 0.0 &bindpid 3 0 1114 1.0 0 &clstime 0.0 &udiepid 3 0 1115 -1.0 0 &endtime &clstime &bindpid 3 0 1115 -1.0 0 &endtime &clstime $---+----1----+----2----+----3----+----4----+----5----+----6----+----7----+----8 *DEFINE_CURVE 1113 0.0,0.0 &clsramp,&vcls &clstime,0.0 *DEFINE_CURVE 1114 0.0,0.0 10.0,0.0 *DEFINE_CURVE 1115 0.0,0.0 &drwramp,&vdraw &drwtime,&vdraw The keyword example below illustrates the use of load curves 3213 and 3124 to specify the states written to the d3plot and intfor files respectively. In addition to the eight states specified by curve 3213, five additional outputs will be generated. Similarly, in addition to the 10 intfor states defined by curve 3214, eight additional states will be output. *CONTROL_FORMING_OUTPUT $ CID NOUT TBEG TEND y1 y2 y3 y4 1113 13 &clstime -3213 *CONTROL_FORMING_OUTPUT_INTFOR $ CID NOUT TBEG TEND y1 y2 y3 y4 1113 18 &clstime -3214 *DEFINE_CURVE 3213 88.0 63.0 42.0 21.5 9.8 5.2 3.1 1.0 *DEFINE_CURVE 3214 74.0 68.0 53.0 32.0 25.5 7.8 4.2 2.1 1.4 0.7 Application example for a multiple flanging process: Referring to Figure 12-36 and a partial keyword example listed below, flanging steels #1 through #4 are defined as parameters &flg1pid through &flg4pid, respectively, which are moving in their own local coordinate systems. The termination time &endtime is defined as pad closing time &clstime plus the maximum travel time of all four flanging steels. A total of ten d3plot states and ten intfor states are defined for each flanging steel using curve IDs 980 and 981, respectively. Curve values outside of the last 10 states (distances) are ignored; and reversed points are automatically adjusted. In Figure 12-37, locations of d3plot states are indicated by “x” markers for each flanging steel move. Note that for flanging steels with longer travel distances, there may be additional d3plot states between the defined points, controlled by distance output defined for other flanging steels with shorter travels. The total number of d3plot (and intfor) states is the sum of all nout defined for each flanging steel so care should be taken to limit the total d3plot (and intfor) states, especially if large number of flanging steels are present. *KEYWORD $ -------------------------closing *BOUNDARY_PRESCRIBED_MOTION_RIGID $ typeID DOF VAD LCID SF VID DEATH BIRTH &upid1 3 0 1113 &padvdir 0 &clstime *BOUNDARY_PRESCRIBED_MOTION_RIGID_local &flg1pid 3 0 1114 1.0 0 &clstime &flg2pid 3 0 1114 1.0 0 &clstime &flg3pid 3 0 1114 1.0 0 &clstime &flg4pid 3 0 1114 1.0 0 &clstime $ -------------------------flanging *BOUNDARY_PRESCRIBED_MOTION_RIGID $ typeID DOF VAD LCID SF VID DEATH BIRTH &upid1 3 0 1115 &padvdir 0 &clstime *BOUNDARY_PRESCRIBED_MOTION_RIGID_local &flg1pid 3 0 1116 1.0 0 &clstime &flg2pid 3 0 1117 1.0 0 &clstime &flg3pid 3 0 1118 1.0 0 &clstime &flg4pid 3 0 1119 1.0 0 &clstime $---+----1----+----2----+----3----+----4----+----5----+----6----+----7----+----8 *DEFINE_CURVE 1116 0.0 0.0 &tdrwup &vdrw &tdown1 &vdrw &drw1tim 0.0 1.0E+20 0.0 *DEFINE_CURVE 1117 0.0 0.0 &tdrwup &vdrw &tdown2 &vdrw &drw2tim 0.0 1.0E+20 0.0 *DEFINE_CURVE 1118 0.0 0.0 &tdrwup &vdrw &tdown3 &vdrw &drw3tim 0.0 1.0E+20 0.0 *DEFINE_CURVE 1119 0.0 0.0 &tdrwup &vdrw &tdown4 &vdrw &drw4tim 0.0 1.0E+20 0.0 $---+----1----+----2----+----3----+----4----+----5----+----6----+----7----+----8 *DEFINE_CURVE 980 60.0 55.0 42.0 40.0 38.0 31.0 23.0 19.0 15.0 13.0 13.5 5.0 3.0 2.0 2.5 1.0 *DEFINE_CURVE 981 23.0 19.0 15.0 13.0 13.5 ⋮ *CONTROL_FORMING_OUTPUT $ -------1---------2---------3---------4---------5---------6---------7---------8 $ CID NOUT TBEG TEND Y1/LCID 1116 10 &clstime &endtime -980 1117 10 &clstime &endtime -980 1118 10 &clstime &endtime -980 1119 10 &clstime &endtime -980 *CONTROL_FORMING_OUTPUT_INTFOR $ -------1---------2---------3---------4---------5---------6---------7---------8 $ CID NOUT TBEG TEND Y1/LCID 1116 10 &clstime &endtime -981 1117 10 &clstime &endtime -981 1118 10 &clstime &endtime -981 1119 10 &clstime &endtime -981 ⋮ ⋮ ⋮ ⋮ ⋮ An example of using CIDT: The example below shows in addition to the 7 states output based on various distances from punch home, defined by load curve 980, 4 more states are output based on simulation time, defined by load curve 999. $---+----1----+----2----+----3----+----4----+----5----+----6----+----7----+----8 *DEFINE_CURVE 999 1.0e-03 2.0e-03 3.0e-03 4.0e-03 *DEFINE_CURVE 980 13.5,0.0 13.0,0.0 5.0,0.0 3.0,0.0 2.5,0.0 2.0,0.0 1.0,0.0 *CONTROL_FORMING_OUTPUT $ -------1---------2---------3---------4---------5---------6---------7---------8 $ CID NOUT TBEG TEND Y1/LCID Y2/CIDT 1116 0 &clstime &endtime -980 -999 1117 0 &clstime &endtime -980 -999 1118 0 &clstime &endtime -980 -999 1119 0 &clstime &endtime -980 -999 Revision information: This feature is available starting from LS-DYNA Revision 74957. Other options’ availabilities are as follows: 7. Y1/LCID is available from Revision 81403. 8. The scale factor SFO for ordinate values in *DEFINE_CURVE is supported from Revision 82755. 9. Output for multiple tools is available from Revision 83090. 10. Support for arbitrary BIRTH and DEATH in *BOUNDARY_PRESCRIBED_MO- TION_RIGID is available from Revision 83090. 11. The INTFOR option is available from Revision 83757. 12. Y2/CIDT is available from Revision 110091. 13. Negative abscissa in the LCID is available starting from Revision 112604. Time = 0.0051966 Time = 0.01366 Binder closing Punch home Figure 12-35. An air draw example with closing and drawing. Flanging steel #4 Flanging steel #3 (hidden behind) Flanging steel #2 Upper pressure pad Flanging steel #1 Figure 12-36. An example of multiple flanging process. Distance to home - &flg4pid: 23.0 15.0 13.0 19.0 13.5 5.0 3.0 2.5 2.0 1.0 &flg1pid &flg2pid &flg3pid &flg4pid ) ( 30 25 20 15 10 0.0 0.002 0.004 0.006 0.008 &endtime Explicit time (sec.) Figure 12-37. D3PLOT/INTFOR output in case of multiple flanging process. *CONTROL_FORMING_PARAMETER_READ Purpose: This feature allows for reading of a numerical number from an existing file and store in a defined parameter. The parameter can be used and referred in the current simulation. The file to be read may be a result from a previous simulation. The file may also simply contain a list of numbers defined beforehand and to be used for the current simulation. Card 1 1 2 3 4 5 6 7 8 Variable Type FILENAME C Parameter Cards. Include one card for each parameter. The next “*” card terminates the input. Card 2 1 2 3 4 5 6 7 8 Variable PARNAME METHOD LINE # BEGIN END Type C Default none I 0 I 0 I 0 I 0 VARIABLE DESCRIPTION FILENAME Name of the file to be read. PARNAME Parameter name. Maximum character length: 7. METHOD Read instruction: EQ.1: read, follow definition by LINE#, BEGIN and END definition LINE # Line number in the file. BEGIN Beginning column number in the line number defined above. END Ending column number in the line number defined above. Remarks: 1. Keyword input order is sensitive. Recommended order is to define variables in *PARAMETER first, followed with this keyword, using the defined variables. 2. Multiple variables can be defined with one such keyword, with the file name needed to be defined only once. If there are variables located in multiple files, the keyword needs to be repeated for each file. 3. An example provided below shows that multiple PIDs for individual tools and blank are defined in files “data.k” and “data1.k”. In the main input file “sim.dyn” used for LS-DYNA execution, variables (integer) are first initialized for PIDS of all tools and blank with *PARAMETER. These variables are updat- ed with integers read from files “data.k” and “data1.k” from respective line number and column number through the use of this keyword. In the *SET_- PART_LIST definition, these PIDs are used to define the part set. Below is file “data.k”, to be read into “sim.dyn:: $$$$$$$$$$$$$$$$$$$$$$$$$ $$$ define PIDs $$$$$$$$$$$$$$$$$$$$$$$$$ $---+----1----+----2----+----3----+----4----+----5----+----6----+----7----+-- upper die pid: 3 lower post pid: 2 Below is file “data1.k”, also to be read into “sim.dyn”: $$$$$$$$$$$$$$$$$$$$$$$$$ $$$$$$$$$$$$$$$$$$$$$$$$$ $$$$$$$$$$$$$$$$$$$$$$$$$ $$$ define PIDs $$$$$$$$$$$$$$$$$$$$$$$$$ $---+----1----+----2----+----3----+----4----+----5----+----6----+----7----+-- lower binder pid: 4 blank pid: 1 Below is partial input for the main input file “sim.dyn”: $---+----1----+----2----+----3----+----4----+----5----+----6----+----7----+-- *INCLUDE blank.k *INCLUDE tool.k $---+----1----+----2----+----3----+----4----+----5----+----6----+----7----+-- *PARAMETER Iblankp,0 Iupdiep,0 Ipunchp,0 Ilbindp,0 Rblankmv,0.0 Rpunchmv,0.0 Rupdiemv,0.0 Rbindmv,0.0 Rbthick,1.6 $---+----1----+----2----+----3----+----4----+----5----+----6----+----7----+-- *CONTROL_FORMING_PARAMETER_READ data.k updiep,1,5,30,30 punchp,1,6,30,30 *CONTROL_FORMING_PARAMETER_READ data1.k lbindp,1,7,30,30 blankp,1,8,30,30 $---+----1----+----2----+----3----+----4----+----5----+----6----+----7----+-- *SET_PART_LIST 1 &blankp *SET_PART_LIST 2 &punchp *SET_PART_LIST 3 &updiep *SET_PART_LIST 4 &lbindp $---+----1----+----2----+----3----+----4----+----5----+----6----+----7----+-- *CONTROL_FORMING_AUTOPOSITION_PARAMETER_SET $# psid cid dir mpsid position premove thick parname 1 0 3 2 1 0.000 &bthick blankmv 3 0 3 1 1 0.000 updiemv 4 0 3 1 -1 0.000 bindmv $---+----1----+----2----+----3----+----4----+----5----+----6----+----7----+-- *PART_MOVE $pid,xmov,ymov,zmov,cid,ifset 1,0.0,0.0,&blankmv,,1 3,0.0,0.0,&updiemv,,1 4,0.0,0.0,&bindmv,,1 4. This feature is available in LS-DYNA R5 Revision 55035 and later releases. *CONTROL_FORMING_POSITION Purpose: This keyword allows user to position tools and a blank in setting up a stamping process simulation. All tools must be pre-positioned at their home positions. For tools that are positioned above the sheet blank (or below the blank) and ready for forming, *CONTROL_FORMING_TRAVEL should be used. This keyword is used together with *CONTROL_FORMING_USER. One *CONTROL_FORMING_POSI- TION card may be needed for each part. NOTE: This option has been deprecated in favor of *CON- TROL_FORMING_AUTOPOSITION_PARAME- TER). Positioning Cards. For each part to be positioned include an additional card. The next “*” card terminates the input. Card 1 1 2 3 4 5 6 7 8 Variable PID PREMOVE TARGET Type I F Default none none I I VARIABLE DESCRIPTION PID Part ID of a tool to be moved, as in *PART The distance to pre-move the tool, in the reverse direction of forming. Target tool PID, as in *PART. The tool (PID) will be moved in the reverse direction of the forming and positioned to clear the interference with the blank, then traveled to its home position with a distance GAP (*CONTROL_FORMING_USER) away from the TARGET tool to complete the forming. PREMOV TARGET Remarks: When this keyword is used, all stamping tools must be in their respective home positions, which is also the position of each tool at its maximum stroke. From the home position each tool will be moved to its start position, clearing interference between the blank and tool yet maintaining the minimum separation needed to avoid initial penetration. Currently the tools can only be moved and travels in the direction of the global Z-axis. A partial keyword example is provided in manual pages under *CONTROL_FORM- ING_USER. Revision information: This feature is available starting in Revision 24641. *CONTROL_FORMING_PRE_BENDING Purpose: This keyword allows for a pre-bending of an initially flat sheet metal blank, typically used in controlling its gravity loaded shape during sheet metal forming. Card 1 1 2 Variable PSET RADIUS Type I F 3 VX F 4 VY F 5 VZ F 6 XC F 7 YC F 8 ZC F Default none none none none none none none none VARIABLE DESCRIPTION PSET Part set ID to be included in the pre-bending. RADIUS Radius of the pre-bending. GT.0.0: bending center is on the same side as the element normals LT.0.0: bending center is on the reverse side of the element normals. See figure below for more information. VX, VY, VZ XC, YC, ZC Vector components of an axis about which the flat blank will be bent. X, Y, Z coordinates of the center of most-bent location. If undefined, center of gravity of the blank will be used as a default. About pre-bending for gravity: In some situation, a flat blank upon gravity loading will result in a “concave” shape in a die. This mostly happens in cases where there is little or no punch support in the middle of the die cavity and in large stamping dies. Although the gravity loaded blank shape is correct the end result is undesirable. In these conditions, buckles may result during the ensuing closing and forming simulation. In reality, a true flat blank rarely exists. Typically, the blank is either manipulated (shaking or bending) by die makers in the tryout stage, or by suction cups in a stamping press, to get an initial convex shape prior to the binder closing and punch forming. This keyword allows this bending to be performed. *CONTROL_FORMING_PRE_BENDING A partial keyword example (NUMISHEET2022 fender outer) is provided below, where blank part set ID variable &BLKSID is defined previously, is to be bent in a radius value of -10000.0mm, with the bending axis of Z, located on the reverse side of the blank positive normal (Figure 12-38). The bending is off gravity center at x = 234.0, y = 161.0, z = 81.6 (to the right along positive X-axis). Only a slight pre-bending on the blank is needed to ensure a convex gravity-loaded shape. *KEYWORD ⋮ *CONTROL_IMPLICIT_FORMING 1 *CONTROL_FORMING_PRE_BENDING $ PSET RADIUS VX VY VZ XC YC ZC &BLKSID -10000. 0.00 0.00 1.0 234.000 161.000 81.60 ... *END In Figures 12-39, initial blank shape without pre-bending is shown. Without pre- bending, the gravity loaded blank sags in the middle of the die cavity, Figure 12-40, which is likely unrealistic, and would lead to predictions of surface quality issues. With pre-bending applied, Figure 12-41, blank bends slight and in convex shape before loading. This shape results in an overall convex shape after gravity completes loading (Figure 12-42), leading to a much shorter binder closing distance, and a more realistic surface quality assessment. Revision information: This feature is available in double precision LS-DYNA Revision 66094 and later releases. It is also available in LS-PrePost4.0 eZ-Setup for metal forming application (http://- ftp.lstc.com/anonymous/outgoing/lsprepost/4.0/metalforming/). Sheet blank normal direction Bending axis Figure 12-38. Negative “R” puts center of bending on the opposite side of the positive blank normal. Sheet blank Lower binder Lower punch Figure 12-39. Initial model before auto-positioning. Blank sags in the die cavity Gravity loaded sheet blank Figure 12-40. Gravity loaded blank without using this keyword. Sheet blank pre-bent with R=10000 mm Figure 12-41. Pre-bending using this keyword (1st state of D3plots). Gravity loaded on pre-bensheet blank Figure 12-42. Gravity loaded shape (last state of D3plots) with convex shape. *CONTROL_FORMING_PROJECTION Purpose: To remove initial penetrations between the blank and the tooling (shell elements only) by projecting the penetrated blank (slave) nodes along a normal direction to the surface of the blank with the specified gap between the node and the tooling surface. This is useful for line die simulation of the previously formed panel to reduce tool travel therefore saving simulation time. Define Projection Card. This card may not be repeated. Card 1 1 2 3 4 5 6 7 8 Variable IDPS IDPM GAP NRSST NRMST Type I I F I I Default VARIABLE DESCRIPTION IDPS IDPM GAP Part ID of the blank (slave side). Part ID for the tool (master side). A distance, which defines the minimum gap required. NRSST Normal direction of the blank: EQ.0: the normal to the surface of the blank is pointing towards the tool, EQ.1: the normal to the surface of the blank is pointing away from the tool. NRMST Normal direction of the tool: EQ.0: the normal to the surface of the tool is pointing towards the blank, EQ.1: the normal to the surface of the tool is pointing away from blank. Remarks: This feature requires consistent normal vectors for both the rigid tooling surface and the blank surface. *CONTROL_FORMING_PROJECTION This feature is available starting in Revision 25588. *CONTROL_FORMING_REMOVE_ADAPTIVE_CONSTRAINTS Purpose: This keyword converts an adaptive mesh into a fully connected mesh. Adaptive constraints are removed and triangular elements are used to connect the mesh. Card 1 1 2 3 4 5 6 7 8 Variable PID Type Default I 0 VARIABLE PID Remarks: DESCRIPTION Part ID (as in *PART) of the part whose adaptive mesh constraints is to be removed and its mesh converted into connected meshes. In some application in sheet metal forming, such as stoning or spirngback simulation, adaptive refinement on the sheet blank may affect the accuracy of the calculation. To avoid this problem, non-adapted mesh is required. However, adaptively refined mesh has the optimal mesh density that is tailored to the tooling geometry; the resulting mesh, in its initial shape, either flat or deformed, has fewer elements (than a blank with non-adapted and uniformly-sized elements) and thus is the most efficient for simulation. If the parameter IOFLAG in *CONTROL_ADAPTIVE is turned on, such a mesh adapt.msh will be generated at the end of each simulation, with its shape conforming to the initial input blank shape. This keyword takes the adapted mesh, removes the adaptive constraints, and use triangular elements to connect the otherwise disconnected mesh. The resulting mesh is a fully connected mesh, with the optimal mesh density, to be used to rerun the simulation (without mesh adaptivity) for a better accuracy. Note that the original adapt.msh file from a LS-DYNA run will include not only the blank but the tooling mesh as well. In order to be used for this keyword, the original file can be read into LS-PrePost, with blank shown in active display only, and menu option File → Save As → Save Active Keyword As can be used to write out the adapted blank mesh only. *CONTROL_FORMING_REMOVE_ADAPTIVE_CONSTRAINTS The following complete input file converts an adaptive mesh file blankadaptmsh.k (Figure 12-43 left) with the PID of 1 into a connected mesh (Figure 12-43 right). The resulting mesh will be in the dynain file. *KEYWORD *INCLUDE blankadaptmsh.k *PARAMETER I blkpid 1 $--------1---------2------- *CONTROL_TERMINATION 0.0 *CONTROL_FORMING_REMOVE_ADAPTIVE_CONSTRAINTS $ PID &blkpid *set_part_list 1 &blkpid *INTERFACE_SPRINGBACK_LSDYNA_NOTHICKNESS 1 *INTERFACE_SPRINGBACK_EXCLUDE INITIAL_STRAIN_SHELL INITIAL_STRESS_SHELL *PART $ PID SID MID &blkpid 1 1 *MAT_037 ... *SECTION_SHELL $ SECID ELFORM SHRF NIP 1 2 0.000E+00 3 1.0,1.0,1.0,1.0 *END Original mesh: adapt.msh Modified, fully connected mesh: dynain Figure 12-43. Converting an adaptive mesh to a fully connected mesh. Revision information: This feature is available starting from LS-DYNA Revision 108157, in both SMP, MPP, single and double precision. *CONTROL_FORMING_SCRAP_FALL Purpose: This keyword allows for direct and aerial trimming of a sheet metal part by trim steels in a trim die. According to the trim steels and trim vectors defined, the sheet metal part will be trimmed into a parent piece and multiple scrap pieces. The parent piece is defined as a fixed rigid body. Trimmed scraps (deformable shells) are constrained along trim edges until they come into contact with the trim steel; the edge constraints are gradually released as the trim steel’s edge contacts the scrap piece, allowing for contact-based scrap fall simulation. This keyword applies to shell elements only. Include Card 1 columns 1-6 only per each scarp piece for the constraint release method . For the scrap trimming method include one set of Cards 1, 2 and 3 per trim steel. The next “*” card terminates the input. Card 1 1 2 3 4 5 6 7 8 Variable PID VECTID NDSET LCID DEPTH DIST IDRGD IFSEED Type I I I I F F I I Default none none none none none none none none Card 2 1 2 3 4 5 6 7 8 Variable NOBEAD SEEDX SEEDY SEEDZ EFFSET GAP IPSET EXTEND Type I F F F F F I F Default none none none none none none none none Card 3 1 2 3 4 5 6 7 8 Variable NEWID Type I Default none VARIABLE PID VECTID NDSET DESCRIPTION Part ID of a scrap piece. This part ID becomes a dummy ID if all trimmed scrap pieces are defined by NEWID. See definition for NEWID and Figure 12-46. Vector ID for a trim steel movement, as defined by *DEFINE_- VECTOR. If left undefined (blank), global 𝑧-direction is assumed. A node set consists of all nodes along the cutting edge of the trim steel. Note that prior to Revision 90339 the nodes in the set must be defined in consecutive order. See Remarks (LS- PrePost) below on how to define a node set along a path in LS- PrePost. This node set, together with VECTID, is projected to the sheet metal to form a trim curve. To trim a scrap out of a parent piece involving a neighboring trim steel, which also serves as a scrap cutter, the node set needs to be defined for the scrap cutter portion only for the scrap, see Figure 12-46. LCID Load curve ID governing the trim steel kinematics, as defined by *DEFINE_CURVE. DEPTH DIST IDRGD GT.0: velocity-controlled kinematics LT.0: displacement-controlled kinematics An example input deck is provided below. A small penetrating distance between the cutting edge of the trim steel and the scrap piece, as shown in Figure 12-45. Nodes along the scrap edge are released from automatically added constraints at the simulation start and are free to move after this distance is reached. A distance tolerance measured in the plane normal to the trim steel moving direction, between nodes along the cutting edge of the trim steel defined by NDSET and nodes along an edge of the scrap, as shown in Figure 12-44. This tolerance is used to determine if the constraints need to be added at the simulation start to the nodes along the trim edge of the scrap piece. Part ID of a parent piece, which is the remaining sheet metal after the scrap is successfully trimmed out of a large sheet metal. Note the usual *PART needs to be defined somewhere in the input deck, along with *MAT_20 and totally fixed translational and rotational DOFs. See Figure 12-46. VARIABLE DESCRIPTION IFSEED A flag to indicate the location of the scrap piece. EQ.0: automatically determined. The trim steel defined will be responsible to trim as well as to push (have contact with) the scrap piece. EQ.1: automatically determined, however, the trim steel in definition will only be used to trim out the scrap, not to push (have contact with) the scrap piece. EQ.-1: user specified by defining SEEDX, SEEDY, and SEEDZ A node set to be excluded from initially imposed constraints after trimming. This node set typically consists of nodes in the scrap draw bead region where due to modeling problems the beads on the scrap initially interfere with the beads on the rigid tooling; it causes scrap to get stuck later in the simulation if left as is. See Figure 12-47. NDBEAD SEEDX, SEEDY, SEEDZ 𝑥, 𝑦, 𝑧 coordinates of the seed node on the scrap side; define only when IFSEED is set to “-1”. See Figure 12-46. EFFSET GAP IPSET Scrap edge offset amount away from the trim steel edge, towards the scrap seed node side. This is useful to remove initial interference between the trimmed scrap (because of poorly modeled trim steel) and coarsely modeled lower trim post. See Figure 12-46. Scrap piece offset amount from the part set defined by IPSET (e.g. top surfaces of the scrap cutters), in the direction of the element normals of the IPSET. This parameter makes it easier to remove initial interference between the scrap and other die components. See Figure 12-48. A part set ID from which the scrap will be offset to remove the initial interference, works together only with GAP. The part set ID should only include portions of tool parts that are directly underneath the scrap (top surface portion of the tools). The normals of the IPSET must point toward the scrap. The parts that should belong to IPSET are typically of those elements on the top surface of the scrap cutter, see Figure 12-48. The Scrap piece is modeled as a deform- able shell part; parent piece does not need to be modeled. Trim steel Nodes along the edge of the trim steel are defined in a sequentailly ordered node set. Constraints automatically are generated during initilization for the nodes in blue along the scrap trim edge, according to DIST. GAP > 0.5 × (scrap thickness + shell thickness of trim post) Trim post Trim line DIST Figure 12-44. Modeling details of the constraint release method. Drawing modified from the original sketches courtesy of the Ford Motor Company. VARIABLE EXTEND NEWID Background: DESCRIPTION An amount to extend a trim steel’s edge based on the NDSET defined, so it can form a continuous trim line together with a neighboring trim steel, whose edge may also be extended, to trim out the scrap piece. See Figure 12-46. New part ID of a scrap piece for the scrap area defined by the seed location. If this is not defined (left blank) or input as “0”, the scrap piece will retain original PID as its part ID. See Figure 12-46. This is useful in case where one original scrap is trimmed into multiple smaller pieces, and contacts between these smaller pieces need to be defined. Sheet metal trimming and the resulting scrap fall are top factors in affecting the efficiency of stamping plants worldwide. Difficult trimming conditions, such as those multiple direct trims, a mixture of direct and cam trims, and multiple cam trims involving bypass condition, can cause trimmed scraps to get stuck around and never separate from the trim edge of the upper trim steels or lower trim post. Inappropriate design of die structure and scrap chute can slow down or prevent scraps from tumbling out to the scrap collectors. Smaller scrap pieces (especially aluminum) can sometimes shoot straight up, and get stuck and gather in areas of the die structure. All these problems result in shutdowns of stamping presses, reducing stroke-per-minute (SPM) and causing hundreds of thousands of dollars in lost productivity. With this keyword, engineers can consider the trimming details, manage the scrap trim and the drop energy, study different trimming sequences, explore better die structure and scrap chutes design and layout before a trim die is even built. This feature is developed in conjunction with the Ford Motor Company. The constraint release method: Prior to Revision 91471 , simulating the scrap trim and fall uses the “constraint release” method, where only the scrap piece is modeled and defined. As shown in Figure 12-44, the scrap piece is modeled as a deformable body and the trim steel and trim post as rigid shell elements, while the parent piece does not need to be modeled at all. Between the trim edge of the scrap piece and the post there should be a gap (indicated by GAP in the figure). The gap ensures that the contact interface (to be explained later) correctly accounts for the shell thickness along the edge. A gap that is too small may cause initial penetration between the scrap and the post which may manifest as unphysical adhesion between the scrap and the post. The Scrap piece Trim steel Cutting Tolerance. When a portion of the trim steel comes within DEPTH of a constrained node, the constraint is released. In the above schematic the tolerance is indicated by the highlighted region. Constraint release (final). Last contacted node along the trim line gets released last from the constraints. Trim line Trim post Constraint release (start). First node in contact is the first released from constraints. The motion of the trim steel is carried onto the scrap piece by the contact interface. Figure 12-45. Contact-based separation and contact-driven kinematics and dynamics in the constraint release method. Drawing modified from the original sketches courtesy of the Ford Motor Company. The edge of the scrap piece should initially be flush with that of the trim post (perpendicular to the trim direction), just as exactly what happens in the production environment. If the scrap is unrealistically positioned above the trim post edge, the scrap may be permanently caught between the trim steel and the post under a combination of uncertain trimming forces as the trim steel moves down. During initialization, constraints are added automatically on the nodes along the scrap trim edge corresponding to the node set (NDSET) along the trim steel, based on the supplied tolerance variable DIST and trim vector VECTID. Although the direction of the path is not important, prior to Revision 90339, the NDSET must be arranged so that the nodes are in a sequential order (LS-PrePost 4.0 creating node set by path). As the edge of the trim steel comes within DEPTH distance of the trim line, the constraints are removed. The contact interfaces serve to project the motion of the trim steel onto the scrap piece, see Figure 12-45. The scrap trimming method: The original simplified method has the following drawbacks: 1. No scrap trimming – the scrap piece cannot be trimmed directly from a parent piece; an exact scrap piece after trimming must be modeled. 2. Poorly (or coarsely) modeled draw beads in the scrap piece do not fit properly in badly modeled draw beads on the tooling, resulting in initial interferences between the two and therefore affecting the simulation results. 3. For poorly (or coarsely) modeled scrap edges and trim posts, users have to manually modify the scrap trim edges to clear the initial interference with the trim posts. 4. Users must clear all other initial interferences (e.g. between scrap and scrap cutter) manually. Based on users’ feedback, a new method “scrap trimming” (after Revision 91471) has been developed to address the above issues and to, furthermore, reduce the effort involved in preparing the model. The new method (Figure 12-46) involves trimming scrap from an initially large piece of sheet metal, leaving the parent piece as a fixed rigid body. The trim lines are obtained from the trim steel edge node set NDSET and the trim vector VECTID. Parameters related to the constraint release method: 1. The value of DEPTH is typically set to one-half of the scrap thickness. 2. The initial gap separating the scrap from the post must be greater than the average of the scrap and post thickness values, see Figure 12-44. 3. The input parameter DIST should be set larger than the maximum distance between nodes along the trim steel edge and scrap edge in the view along the trim direction, see Figure 12-44. Parameters related to the scrap trimming method: 4. Similar to DEPTH, EFFSET should be typically set to one-half of the scrap thickness, although it may be larger for some poorly modeled trim steels and trim posts. Contact: Only *CONTACT_FORMING contact interfaces are allowed for contact between the scrap piece and the trim steel. In particular, *CONTACT_FORMING_SURFACE_TO_- SURFACE is recommended. A negative contact offset must be used; this is done typically by setting the variable MST in *CONTACT_FORMING_SURFACE_TO_SUR- FACE to the negative thickness value of the scrap piece. For contact between the scrap piece and the shell elements in all the other die structures, *CONTACT_AUTOMATIC_GENERAL should be used for the edge-to-edge contact frequently encountered during the fall of the scrap piece. All friction coefficients should be small. The explicit time integrator is recommended for the modeling of scrap trim and fall. Mass scaling is not recommended. LS-PrePost: The node set (NDSET) defined along the trim steel edge can be created with LS-PrePost 4.0, via Model/CreEnt/Cre, Set Data, *SET_NODE, ByPath, then select nodes along the trim edge continuously until finish and then hit Apply. Keyword examples – the constraint release method: A partial example of using the keyword below includes a node set ID 9991 along the trim steel (PID 2) edge used to release the constraints between the scrap piece with PID 1, and the parent piece. The LCID for the trim steel kinematics is (+)33 (load curve is controlled by velocity) moving in –Z direction. The trimming velocity is defined as 1000 mm/s and the retracting velocity is 4000 mm/s. The variables DEPTH and DIST are set to 0.01 and 2.5, respectively. The contact interface between the trim steel and scrap piece is defined using *CONTACT_FORMING_SURFACE_TO_SURFACE and contact between the scrap and all other die structures are defined using *CONTACT_- AUTOMATIC_GENERAL. *KEYWORD *CONTROL_TERMINATION &endtime *CONTROL_FORMING_SCRAP_FALL $ PID VECTID NDSET LCID DEPTH DIST 1 9991 33 0.75 2.0 *SET_NODE_LIST 9991 24592 24591 24590 24589 24593 24594 24595 24596 *BOUNDARY_PRESCRIBED_MOTION_rigid $pid,dof,vad,lcid,sf,vid,dt,bt 2,3,0,33,-1.0 *DEFINE_CURVE 33 0.0,0.0 0.216,1000.0 0.31,-4000.0 0.32,0.0 0.5,0.0 $---+----1----+----2----+----3----+----4----+----5----+----6----+----7----+----8 *CONTACT_forming_surface_to_surface_ID 1 1 2 3 3 0 0 0 0 0.02 0.0 0.0 0.0 20.0 0 0.01.0000E+20 $# sfs sfm sst mst sfst sfmt fsf vsf 0.0 0.0 0.0 &mst 1.0 1.0 1.0 1.0 $---+----1----+----2----+----3----+----4----+----5----+----6----+----7----+----8 *CONTACT_AUTOMATIC_GENERAL_ID 2 *END For the negative option of LCID, displacement will be used as input to control the tool kinematics. A partial example is provided below, where LCID is defined as a negative integer of a load curve, controlling the trim steel kinematics. The trim steel is moving down for 27.6075 mm in 0.2 sec to trim, and moving up for the same distance to its original position in 0.3 sec to retract. Although this option is easier to use, the corresponding velocity from the input time and displacement must be realistic for a realistic simulation. *CONTROL_FORMING_SCRAP_FALL $ LCID<0: trimming steel kinematics is controlled by displacement. $ PID VECTID NDSET LCID DEPTH DIST 1 44 1 -33332 0.70 2.00 *DEFINE_VECTOR 44,587.5,422.093,733.083,471.104,380.456,681.412 *BOUNDARY_PRESCRIBED_MOTION_rigid_LOCAL $pid,dof,vad,lcid,sf,vid,dt,bt 11,3,2,33332,1.0,44 *DEFINE_CURVE 33332 0.0,0.0 0.2,-27.6075 0.5,0.0 A keyword example – the scrap trimming method: The keyword example below shows three scrap pieces, with original PID &SPID1, new PIDs 1001 and 1002, being trimmed out of a larger scrap &SPID1; the remaining parent piece is defined as a fixed rigid body with PID 110. A different seed location is defined separately for each scrap. The scraps &SPID1, 1001 and 1002 are each offset by 0.60mm in the area of the seed location defined, in the direction normal to the elements defined by IPSET 887, 888, and 889, respectively. The trim edge offset is 0.90mm for all scraps. The draw bead node sets to be released are, 987, 988, 989 for each scrap as defined by the corresponding seed locations. *CONTROL_FORMING_SCRAP_FALL $ PID VECTID NDSET VLCID DEPTH DIST IDRGD IFSEED &spid1 &cord1 &nset1 1800 &depth1 2.00 110 -1 $ NDBEAD seedx seedy seedz effset GAP IPSET EXTEND 987 -528.046 373.40 710.000 0.90 0.60 887 8.0 0 &spid1 &cord2 &nset2 1801 &depth1 2.00 110 -1 987 -528.046 373.40 710.000 0.90 0.60 887 8.0 0 &spid1 &cord3 &nset3 1802 &depth1 2.00 110 -1 987 -528.046 373.40 710.000 0.90 0.60 887 8.0 0 $ &spid1 &cord3 &nset33 1802 &depth1 2.00 110 -1 988 -252.452 383.322 799.974 0.90 0.60 888 8.0 1001 &spid1 &cord4 &nset4 1803 &depth1 2.00 110 -1 988 -252.452 383.322 799.974 0.90 0.60 888 8.0 1001 &spid1 &cord5 &nset5 1804 &depth1 2.00 110 -1 988 -252.452 383.322 799.974 0.90 0.60 888 8.0 1001 $ &spid1 &cord5 &nset55 1804 &depth1 2.00 110 -1 989 74.452 404.522 857.974 0.90 0.60 889 8.0 1002 &spid1 &cord6 &nset6 1805 &depth1 2.00 110 -1 989 74.452 404.522 857.974 0.90 0.60 889 8.0 1002 &spid1 &cord7 &nset7 1806 &depth1 2.00 110 -1 989 74.452 404.522 857.974 0.90 0.60 889 8.0 1002 Revision/Other information: A graphical user interface capable of setting up a complete input deck for the original simplified method is now available in LS-PrePost 4.0 under APPLICATION/Scrap Trim reference paper (http://ftp.lstc.com/anonymous/outgoing/lsprepost/4.1/). regarding the development and application of this keyword for the constraint release method can be found in the proceedings of the 12th International LS-DYNA User's Conference. The following provides a list of revision history for the keyword: A 1. The constraint release method is available between LS-DYNA Revision 63618 and 91471. 2. The scrap trimming method is available starting in Revision 91471. 3. The parameter NEWID is available starting in Revision 92578. 4. The restriction of NDSET must be defined in a consecutive order is lifted starting in Revision 90339. IDRGD Trim steel 1 Trim steel 2 NEWID2 NEWID1 or PID NEWID3 Scrap cutter Scrap seed node EXTEND EXTEND IDRGD NSET1 Trim steel 1 NEWID2 EFFSET NSET2 SEEDX, Y, Z Trim steel 2 Figure 12-46. Trimming of multiple scraps and parameter definitions in the scrap trimming method. Model courtesy of the Ford Motor Company. NDBEAD NDBEAD Figure 12-47. Definition of NDBEAD in the scrap trimming method. Model courtesy of the Ford Motor Company. Scrap piece Scrap cutter top surface Before trim Scrap cutter side view Element normals Scrap piece: Normals should face the IPSET GAP IPSET: To get the proper offset, elements immediately below the scrap piece should be separated into a different PID (and included in the IPSET) from the vertical walls of the scrap cutter. In addition, IPSET should have consistent normals pointing toward the scrap piece. After trim Figure 12-48. Element normal of the IPSET in the scrap trimming method. Model courtesy of the Ford Motor Company. *CONTROL_FORMING_SHELL_TO_TSHELL Purpose: This keyword is created to allow users to easily change the element type from thin shell elements (*SECTION_SHELL) to thick shell elements (*SECTION_TSHELL), and to generate segments on both top and bottom side of the thick shells. Note that mesh adaptivity is also supported. Card 1 1 2 3 4 5 6 7 8 Variable PID THICK MIDSF IDSEGB IDSEGT Type I I I I I Default none none none none none VARIABLE DESCRIPTION PID Part ID of the thin shell elements. THICK Thickness of the thick shell elements (Tshell). MIDSF Tshell mid-plane position definition : IDSEGB MIDSF.EQ.0: Mid-plane is at thin shell surface. MIDSF.EQ.1: Mid-plane is at one half of THICK above thin shell surface. MIDSF.EQ.-1: Mid-plane is at one half of THICK below thin shell surface. Set ID of the segments to be generated on the bottom layer of the Tshells, which can be used for segment-based contact. The bottom side of Tshells is the opposite side of the positive normal side of the thin shells, see Figure 12-49. Note the default normal of the generated segments are consistent with the thin shells’ normal. To reverse this default normal, set the IDSEGB to a negative number. Under the FORMING type of contact, if the generated segments are used as a slave member in contact with a master member of a rigid body, the rigid body’s normals must be consistent and facing the slave segments. Note that the slave segments normals are not required to point at the rigid bodies, although they should be made consistent. IDSEGT *CONTROL_FORMING_SHELL_TO_TSHELL DESCRIPTION Set ID of the segments to be generated on the top layer of the Tshells, which can be used for segment-based contact. The top side of a Tshells is the same side of the positive normal side of the thin shells, see Figure 12-49. Note the normal of the generated segments are consistent with the thin shells’ normal. To reverse this default normal, set the IDSEGT to a negative number. Remarks: This keyword will convert thin shell elements to thick shell elements. The position of the thick shells’ mid-plane in reference to the thin shell’s surface is dependent on MIDSF (Figure 12-49). Node IDs of the thick shell elements will be the same as those for the thin shells. Element IDs of the thick shell elements will start at 2 (so renumber element IDs of other PID accordingly). Only one layer of thick shells will be created. New nodes generated adaptively from their parent nodes with *BOUNDARY_SPC are automatically constrained accordingly. This feature is developed as requested by JSOL Corporation. Examples: 1)A standalone part of thin shell elements can be changed to thick shell elements with a simplified small input deck. The following will convert shell elements with PID 100 of thickness 1.5mm to thick shell elements of PID 100 with thick- ness of 2.0mm, with thick shell meshes stored in a file “dynain.geo”. Note that MIDSF, IDSEGB and IDSEGT cannot be used in this case. *KEYWORD *CONTROL_TERMINATION 0.0 *INCLUDE shellupr.k *SET_PART_LIST 1, 100 *PART Sheet blank 100,100,100 *SECTION_SHELL $ SID ELFORM SHRF NIP PROPT 100 2 0.833 3 1.0 $ T1 T2 T3 T4 NLOC 1.5,1.5,1.5,1.5 *MAT_037 $# MID RO E PR SIGY ETAN R HLCID 100 7.8500E-9 2.1000E+5 0.333000 1.00 90905 *DEFINE_CURVE 90905 0.000000000E+00 0.380000000E+03 0.300000003E-02 0.392489226E+03 0.600000005E-02 0.403294737E+03 0.899999961E-02 0.412847886E+03 0.120000001E-01 0.421429900E+03 0.150000006E-01 0.429234916E+03 0.179999992E-01 0.436402911E+03 0.209999997E-01 0.443038343E+03 *INTERFACE_SPRINGBACK_LSDYNA 1 OPTCARD,,,1 *CONTROL_FORMING_SHELL_TO_TSHELL $ PID THICK 100 2.0 *END that 2)The conversion can also be done in an input deck set up for a complete metal forming simulation with thin shell elements as a sheet blank. The conversion happens in the beginning of the simulation, as shown in an example below. Only the keywords needed change are listed, commented out with $ signs and replaced with appropriate cards for thick shells. The thin shell sheet blank with PID 1 is to be converted to a thick shell sheet blank with thickness of 1.6mm, noting instead of *SECTION_SHELL for the sheet blank. Corresponding material type for the sheet blank (*MAT_037) also needs to be changed to a type that supports solid element simulation (*MAT_024). The mid-plane of the thick shells will be one half of 1.6 mm below the thin shells’ surface, with segment IDs 10 (IDSEGB) and 11 (IDSEGT) created on the bottom and top side of the thick shells, respectively, as shown in Figure 12-49. IDSEGB 10 with SSTYP 0 is defined to contact with the lower punch (part set ID 2) with MSTYP 2, and IDSEGT 11 with SSTYP 0 is used for contact with the upper die cavity with part set ID of 3, of MSTYP 2. should be defined *SECTION_TSHELL the *KEYWORD ... *PART Sheet blank 1,1,1 $---+----1----+----2----+----3----+----4----+----5----+----6----+----7----+----8 $ Blank property $---+----1----+----2----+----3----+----4----+----5----+----6----+----7----+----8 $*SECTION_SHELL $ SID elform SHRF nip PROPT QR/IRID ICOMP SETYP $ 1 2 0.833 3 1.0 $ T1 T2 T3 T4 NLOC $&b1thick,&b1thick,&b1thick,&b1thick *SECTION_TSHELL $ SID elform SHRF nip PROPT QR/IRID ICOMP SETYP 1 1 0.833 &nip 1.0 $---+----1----+----2----+----3----+----4----+----5----+----6----+----7----+----8 $*MAT_037 $ MID RO E PR SIGY ETAN R HLCID $ 1 7.85E-09 2.07E+05 0.28 92 *MAT_024 $ MID RO E PR SIGY ETAN FAIL TDEL 1 7.85E-09 2.07E+05 0.28 382.8 0.0 0.0 0.0 $ C P LCSS LCSR VP 0.0 0.0 92 0 0.0 $ EPS1 EPS2 EPS3 EPS4 EPS5 EPS6 EPS7 EPS8 $ ES1 ES2 ES3 ES4 ES5 ES6 ES7 ES8 *DEFINE_CURVE 92,,,0.5 0.0000000000E+00 3.8276000000E+02 4.0000000000E-03 3.9616000000E+02 8.0000000000E-03 4.0695000000E+02 ⋮ ⋮ *INTERFACE_SPRINGBACK_LSDYNA 1 OPTCARD,,,1 *CONTROL_FORMING_SHELL_TO_TSHELL $ PID THICK MIDSF IDSEGB IDSEGT 100 1.6 -1 10 11 *CONTACT_FORMING_ONE_WAY_SURFACE_TO_SURFACE $ SSID MSID SSTYP MSTYP 11 2 0 2 ⋮ ⋮ ⋮ *CONTACT_FORMING_ONE_WAY_SURFACE_TO_SURFACE $ SSID MSID SSTYP MSTYP 10 3 0 2 ⋮ ⋮ ⋮ ... *END Revision information: This feature is available in LS-DYNA starting in Revision 104903. The following revisions indicate the Revision history of additional features: 1) Revision 106116: negative option of IDSEGB and IDSEGT. 2) Revision 106162: MIDSF, IDSETGB and IDSEGT becomes available. 3) Revision: 106217: automatically add *BOUNDARY_SPC for newly generated nodes whose parent nodes are assigned with *BOUNDARY_SPC. Thin shell normals Original sheet blank with shell elements Thin shell surface Created thick shells for MIDSF=0 Thick shell mid-plane THICK THICK THICK Created thick shells for MIDSF=1 Thick shell mid-plane Created thick shells for MIDSF=-1 Thick shell mid-plane NUMISHEET'05 Cross member Top segment ID 11 (IDSEGT) Bottom segment ID 10 (IDSEGB) Figure 12-49. Converting thin shells to thick shells in sheet metal forming *CONTROL_FORMING_STONING Purpose: This feature is developed to detect surface lows or surface defects formed during metal stamping. This calculation is typically performed after a springback simulation. A curvature-based method is implemented with the feature. Users have the option to check an entire part or just a few local areas, defined by node set or shell element set. In each area, direction of the stoning action can be specified by two nodes or simply allow the program to automatically determine the stoning direction. Card 1 1 2 3 4 5 6 7 8 Variable ISTONE LENGTH WIDTH STEP DIRECT REVERSE METHOD Type I F F F F Default none 0.0 0.0 0.0 0.0 Card 2 1 2 3 4 Variable NODE1 NODE2 SID ITYPE Type Default I 0 I 0 I 0 I 0 5 V1 F 0.0 0.0 0.0 I 0 6 V2 F I 0 7 V3 F 8 VARIABLE DESCRIPTION ISTONE Stoning calculation option. EQ.1: calculate panel surface quality using stoning method. LENGTH Length of the stone. WIDTH Width of the stone. STEP Stepping size of the moving stone. DIRECT Number of automatically determined stoning direction(s). VARIABLE DESCRIPTION REVERSE Surface normal reversing option: EQ.0: do not reverse surface normals. EQ.1: reverse surface normals. METHOD Stoning method. EQ.0: curvature-based method. NODE1 Tail node defining stoning moving direction. NODE2 Head node defining stoning moving direction. SID Node or shell set ID. ITYPE Set type designation: EQ.1: node set EQ.2: element set V1, V2, V3 Vector components defining stoning direction (optional). About stoning: Stoning is a quality checking process on class-A exterior stamping panels. Typically the long and wider surfaces of an oil stone of a brick shape are used to slide and scratch in a given direction against a localized area of concern on a stamped panel. Surface “lows” are shown where scratch marks are not visible and “highs” are shown in a form of scratch marks. This keyword is capable of predicting both the surface “lows” and “highs”. Since stoning process is carried out after the stamping (either drawn or trimmed) panels are removed from the stamping dies, a springback simulation needs to be performed prior to conducting a stoning analysis. Modeling guidelines: As a reference, typical stone length and width can be set at 150.0 and 30.0 mm, respectively. The step size of the moving stone is typically set about the same order of magnitude of the element length. The smallest element length can be selected as the step size. The variable DIRECT allows for the automatic definition of the stoning directions. Any number can be selected but typically 2 is used. Although CPU time required for the stoning calculation is trivial, a larger DIRECT consumes more CPU time. Stoning is performed on the outward normal side of the mesh. Element normals must be consistent and oriented accordingly. Element normal can be automatically made consistent in LS-PrePost4.0 under EleTol/Normal menu. Alternatively, the variable REVERSE provides in the solver an easy way to reverse a part with consistent element normals before the computation. The variables NODE1 and NODE2 are used to define a specific stoning direction. The stone is moved in the direction defined by NODE1 to NODE2. Alternatively, one can leave NODE1 and NODE2 blank and define the number of automatically determined stoning directions by using the variable DIRECT. Furthermore, stoning direction can also be defined using a vector by defining the variables V1, V2, and V3. The blank model intended for analysis can be included using keyword *INCLUDE. If nothing is defined for SID and ITYPE then the entire blank model included will be used for stoning analysis. A large area mesh can be included in the input file. An ELSET must also be included, which defines a local area that requires stoning computation. Alternatively, an ELSET can define several local areas to be used for the computation. Furthermore, an ELSET should not include meshes that have reversed curvatures. An ELSET can be easily generated using LS-PrePost4.0, under Model/CreEnt/Cre/Set_Data/*SET_SHELL. Since stoning requires high level of accuracy in springback prediction, it is recommended that the SMOOTH option in keyword *CONTACT_FORMING_ONE_- WAY_SURFACE_TO_SURFACE to be used during the draw forming simulation. Not all areas require SMOOTH contact, only areas of interest may apply. In addition, meshes in the areas of concern need to be very fine, with average element size of 1 to 2 mm. Mesh adaptivity is not recommended in the SMOOTH/stoning areas. Also, mass scaling with DT2MS needs to be sufficiently small to reduce the dynamic effect during forming. For binder closing of large exterior panels, implicit static method using *CON- TROL_IMPLICIT_FORMING type 2 is recommended, to further reduce potential buckles caused by the inertia effect. Stoning results/output: It is recommended that double precision version of LS-DYNA be used for this application. The output of the stoning simulation results is in a file named “filename.output”, where “filename” is the name of the LS-DYNA stoning input file containing this keyword, without the file extension. The stoning results can be viewed using LS-PrePost4.0, under MFPost/FCOMP/Shell_Thickness. Application example: An example of a stoning analysis on a Ford Econoline door outer panel is provided for reference. The original part model comes from National Crash Analysis Center at The George Washington University. The original part was modified heavily in LS-PrePost4.0 to fit the needs of the demonstration purpose. Binder and addendum were created and sheet blank size was assumed. The blank is assigned 0.65mm thickness and a BH210 properties with *MAT_037. Shell thickness contour plots for the drawn and trimmed panels are shown in Figures 12-50 and 12-51, respectively. Springback amount in Z is plotted in Figure 12-52. The complete input deck used for the stoning simulation is provided below for reference; where, a local area mesh of the door handle after springback simulation “Doorhandle.k” and an element set “elset1.k” are included in the deck. Locations of the ELSETs are defined for the upper right (Figure 12-53 left) and lower right corners (Figure 12-54 left) of the door handle, where “mouse ear” are expected. *KEYWORD *TITLE Stoning Analysis *INCLUDE Doorhandle.k *INCLUDE elset1.k *CONTROL_FORMING_STONING $ ISTONE LENGTH WIDTH STEP DIRECT REVERSE METHOD 1 150.0 4.0 1.0 9 0 0 $ NODE1 NODE2 SID ITYPE 1 2 *END Stoning results are shown in Figures 12-53 (right) and 12-54 (right) for the upper right and lower right corners, respectively. “Mouse ears” are predicted where anticipated. Revision information: The stoning feature is available in LS-DYNA Revision 54398 and later releases. Vector component option is available in Revision 60829 and later releases. Thickness (mm) 0.6818 0.6649 0.6480 0.6310 0.6141 0.5972 0.5803 0.5634 0.5464 0.5295 0.5126 Figure 12-50. Thickness contour of the panel after draw simulation. Thickness (mm) 0.6818 0.6649 0.6480 0.6310 0.6141 0.5972 0.5803 0.5634 0.5464 0.5295 0.5126 Figure 12-51. Thickness contour of the panel after trimming. Springback (mm) 0.6818 0.6649 0.6480 0.6310 0.6141 0.5972 0.5803 0.5634 0.5464 0.5295 0.5126 Figure 12-52. Springback amount (mm). A region where an "elset" was selected for stoning Stoning results: "mouse ear" potential in the corner Out-of-plane displacement (mm) 0.2336 0.2103 0.1869 0.1636 0.1402 0.1166 0.0935 0.0070 0.0467 0.0234 0.0000 Figure 12-53. Stoning simulation for the upper right door corner. Out-of-plane displacement (mm) 0.3580 0.3222 0.2864 0.2506 0.2148 0.1790 0.1432 0.1074 0.0716 0.0358 0.0000 A region where another "elset" was defined for stoning Stoning results: "mouse ear" potential in the corner Figure 12-54. Stoning simulation for the lower right door corner. *CONTROL_FORMING_TEMPLATE Purpose: This keyword is used to simplify the required input for sheet metal stamping simulations. With this keyword, five templates are given: three-piece air draw, three- piece toggle draw, four-piece stretch draw, trimming, and springback. NOTE: This option has been deprecated in favor of *CON- TROL_FORMING_AUTOPOSITION_PARAME- TER. Card 1 1 2 3 4 5 6 7 8 Variable IDTEMP BLKID DIEID PNCH BNDU BNDL TYPE PREBD Type I I I I I I Default none none none none none none I 0 F 0.0 Remarks 1 Card 2 1 2 2 3 4 5 Variable LCSS AL/FE R00 R45 R90 Type I C F F F 6 E F 7 8 DENSITY PR F F Default none Fe 1.0 R00 R00 none none none Card 3 Variable Type 1 K F 2 N F 3 4 5 6 MTYP UNIT THICK GAP I F F 8 7 FS F Default none none 37 none 1.1t 0.1 I Card 4 1 2 Variable PATERN VMAX Type Default I 1 F 1000 Card 5 1 2 3 VX F 0 3 4 VY F 0 4 5 VZ F 6 7 8 VID AMAX I F -1 none 1.0e+6 5 6 7 8 Variable LVLADA SIZEADA TIMSADA D3PLT Type Default I 1 F I I none 20 10 VARIABLE DESCRIPTION IDTEMP Type of forming process: EQ.1: 3-piece air-draw (Figure 12-55) EQ.2: 3-piece Toggle-draw (Figure 12-56) EQ.3: 4-piece stretch draw (Figure 12-57) EQ.4: Springback EQ.5: Trimming BLKID Part or part set ID that defines the blank. DIEID Part or part set ID that defines the die. See Figures 12-55, 12-56 and 12-57 for more information PNCHID Part or part set ID that defines the punch. BNDUID Part or part set ID that defines the upper binder. BNDLID Part or part set ID that defines the lower binder. Upper die (cavity) Blank Punch (post) Lower binder Binder gap (a) Positioning (b) Binder closing (c) Forming Figure 12-55. IDTEMP = 1: forming in 3-piece air draw. Upper binder Punch (Post) Blank Lower die (cavity) Binder gap (a) Positioning (b) Binder closing (c) Forming Figure 12-56. IDTEMP = 2: forming in 3-piece toggle draw. VARIABLE TYPE DESCRIPTION Flag for part or part set ID used in the definition of BLKID, DIEID, PNCHID, BNDUID, and BNDLID: EQ.0: Part ID EQ.1: Part set ID PREBD LCSS “Pull-over” distance, for 4 piece stretch draw only. This is the travel distance of both upper and lower binder together after they are fully closed. Typically this distance is below 50mm. See Figure 12-57 for more information. If the material (*MAT_XXX) for the blank is not defined, this curve ID will define the stress-strain relationship; otherwise, this curve is ignored. Upper punch Blank Lower die (cavity) Upper binder Lower binder Binder gap PREBD (a) Positioning (b) Binder closing (c) Pull-over (d) Upper closing (e) Draw home Figure 12-57. IDTEMP = 3: forming in 4-piece stretch draw. VARIABLE AL/FE DESCRIPTION This parameter is used to define the Young’s Modulus and density of the blank. If this parameter is defined, E and DENSITY will be defined in the units given by Table 12-58. EQ.A: the blank is aluminum EQ.F: the blank is steel (default) R00, R45, R90 Material anisotropic parameters. For transversely anisotropy the R value is set to the average value of R00, R45, and R90. E Young’s Modulus. If AL/FE is user defined, E is unnecessary DENSITY Material density of blank. If AL/FE is user defined, this parameter is unnecessary PR K Poisson’s ratio. Strength coefficient for exponential hardening (𝜎̅̅̅̅̅ = 𝑘𝜀̅ 𝑛). If LCSS is defined, or if a blank material is user defined by *MAT_XXX, this parameter is ignored. VARIABLE DESCRIPTION N MTYP UNIT THICK GAP Exponent for exponential hardening (𝜎̅̅̅̅̅ = 𝑘𝜀̅ 𝑛). If LCSS is defined, or if a blank material user defined, this parameter is ignored. Only material models *MAT_036 and *MAT_037 are supported. Define a number between 1 and 10 (Table 12-58) to indicate the UNIT used in this simulation. This unit is used to obtain proper punch velocity, acceleration, time step, and material properties. Blank thickness. If the blank thickness is already defined with *SECTION_SHELL, this parameter is ignored. The gap between rigid tools at their home position. If *BOUND- ARY_PRESCRIBED_RIGID_BODY is user defined, this parameter is ignored. The default is 1.1 x blank thickness. FS Friction coefficient (default = 0.10). If the contact (*CONTACT) is user defined, this parameter is ignored. PATERN Velocity profile of moving tool. If the velocity is user defined by *BOUNDARY_PRESCRIBED_RIGID_BODY, PATERN is ignored. EQ.1: Ramped velocity profile EQ.2: Smooth velocity curve VX, VY, VZ Vector components defining the direction of movement. The default direction is defined by VID. the punch VID Vector ID defining the direction of the punch movement. This variable overrides the vector components (VX, VY, VZ). If VID and (VX, VY, VZ) are undefined, the punch is assumed to move in the negative z-direction. AMAX The maximum allowable acceleration. LVLADA Maximum adaptive level. SIZEADA Minimum element size permitted in the adaptive mesh. TIMSADA Total number of adaptive steps during the forming simulation. D3PLT The total number of output states in the D3PLOT database. *CONTROL_FORMING_TEMPLATE UNIT 1 2 3 4 5 6 7 8 9 10 Mass Ton Gm Gm Gm Gm Kg Kg Kg Kg Kg Length Mm Mm Mm Cm Cm Mm Cm Cm Cm Time Force S N Ms S Us S Ms Us Ms S N 𝜇N 1e7N Dyne KN 1e10N 1e4N 1e- 2N m S N Table 12-58. Available units for metal stamping simulation. About IDTEMP: When the variable IDTEMP is set to 1, it represents a 3-piece draw in air, as shown in Figure 12-55. When IDTEMP is set to 2, a 3-piece toggle draw is assumed, Figure 12-56. For IDTEMP of 1 or 2, LS-DYNA will automatically position the tools and minimize the punch travel (step a), calculate the binder and punch travel based on the blank thickness and the home gap (step b), set the termination time based on step (a) and (b), define the rigid body motion of the tooling, establish all the contacts between the blank and rigid tools, and, select all necessary control parameters. When IDTEMP is set to 3, a 4-piece stretch draw shown in Figure 12-57 will be followed. The die action goes as follows: after upper binder moves down to fully close with lower binder, both pieces move together down a certain distance (usually ~50mm) to “pull” the blank “over” the lower die, then upper punch closes with the lower die, finally the binders move down together to their home position. Both toggle draw and 4-piece stretch draw are called “double action” processes which suffer from a slower stamping speed. As the metric of “hits per minute” (or “parts per minute”) becomes a stamping industry benchmark for efficiency, these types of draw are becoming less popular (especially the 4-piece stretch draw). Nevertheless, they remain important stamping processes for controlling wrinkles in difficult-to-form panels such as lift gate inners, door inners and floor pans. These two processes are also used in situation where deep drawn panels require draw depth of over 250mm, the usual limit for automatic transfer presses. For all the above IDTEMP values, users do not need to define additional keywords, such as *PART, *CONTROL, *SECTION, *MAT_…, *CONTACT_… (drawbead definition is an exception), and, *BOUNDARY_PRESCRIPTION_RIGID, etc. If any such keyword is defined, automatic default settings will be overridden. When IDTEMP is set to 4, springback Simulation will be conducted. The only additional keyword, *BOUNDARY_SPC_… is needed to specify the constraints in the input deck. When IDTEMP is set to 5, a trimming operation will be performed. The only additional keyword, *DEFINE_CURVE_TRIM, is needed to specify the trim curves in the input deck. Revision information: This feature is available starting in Revision 45901 and later releases. *CONTROL_FORMING_TIPPING Purpose: This keyword is developed to reorient or reposition a part between the stamping dies. In stamping line die simulation, panel tipping and translation between the die stations are frequently required. Typically such transformation involves only a small amount of rotations, e.g. < 15 degrees; and some large amounts of translation. For example, there could be a tipping angle of 10 degree along Y-axis and a translation of 2000 mm along the X-axis between the current trimming die and next flanging die. Card Set. For each rotated or translated part or set add a Tipping Card plus NMOVE Move Cards. The data set for this keyword ends at the next keyword (“*”) card. Tipping Card. Specify a part or set ID to be tipped. Card 1 1 2 3 4 5 6 7 8 Variable PID/SID ITYPE ISTRAIN IFSTRSS NMOVE Type I I Default none none I 0 I 0 I 0 Move Card (Rot). Format when first entry, ROT/TRAN, is set to 1. Card 2 1 2 3 4 5 6 7 8 Variable ROT/TRAN V11 V12 V13 X01 Y01 Z01 DISTA1 Type I F F F F F F F Default none 0.0 0.0 0.0 0.0 0.0 0.0 0.0 Move Card (Trans). Format when first entry, ROT/TRAN, is set to 2. 5 6 7 8 Card 2 1 2 Variable ROT/TRAN DX Type I F 3 DY F 4 DZ F Default none 0.0 0.0 0.0 VARIABLE PID/SID DESCRIPTION Part ID or part set ID of part(s) that requires tipping and/or translation. ITYPE Part ID or part set ID indicator: EQ.1: PID means part ID, EQ.2: PID/SID means part set ID. ISTRAIN Strain tensors inclusion option: EQ.1: include in tipping/translation. ISTRESS Stress tensors inclusion option: EQ.1: include in tipping/translation. NMOVE Total number of tipping and translation intended with this keyword. ROT/TRAN Transformation type: EQ.1: rotation, EQ.2: translation. V11, V12, V13 X01, Y01, Z01 Vector components of an axis about which tipping is performed. X, Y and Z coordinates of a point through which the tipping axis passes. DSITA Tipping angle in degree. DX, DY, DZ Translation distances along global X-axis, Y-axis and Z-axis. *CONTROL_FORMING_TIPPING 1. Keyword *INCLUDE can be used to include the file to be tipped or translated. 2. Tipping angle DISTA1 is defined in degree. Signs of the tipping angles follow the “right hand rule”. 3. An example of the keyword is included below, to tip a part +23.0 degrees, -31.0 degrees, and +8.0 degrees about X-, Y-, and Z-axis, respectively and passing through the origin; and to translate the part 12.0mm, -6.0mm and 91.0mm along X, Y, and Z axis, respectively. *INCLUDE trimmedpart.dynain *CONTROL_FORMING_TIPPING $ PID/PSID ITYPE ISTRAIN ISTRSS NMOVE 1 0 1 1 4 $ ROT/TRAN V11 V12 V13 X01 y01 z01 DSITA1 1 1.000 0.000000 0.000 0.000 0.000 0.000 23.0 $ ROT/TRAN V21 V22 V23 X21 y21 z21 DSITA2 1 0.000 1.000000 0.000 0.000 0.000 0.000 -31.0 $ ROT/TRAN V31 V32 V33 X31 y31 z31 DSITA3 1 0.000000 0.000 1.000 0.000 0.000 0.000 8.0 $ ROT/TRAN DX DY DZ 2 12.0 -6.0 91.0 Revision Information: This feature is available starting in LS-DYNA Revision 53448, with major updates from Revision 80261. It is also available in LS-PrePost4.0 eZSetup for metal forming application (http://ftp.lstc.com/anonymous/outgoing/lsprepost/4.0/metalforming/). *CONTROL_FORMING_TOLERANC Purpose: This keyword utilizes a smoothing algorithm to reduce the output noise of the strain ratio β (minor strain/major strain) in calculating the Formability Index (F.I.), which predicts sheet metal failure under nonlinear strain paths frequently occurred in metal forming application. This keyword must be used together with the NLP option in and for *MAT_036 and *MAT_037 only; and applies to shell elements only. This feature is jointly developed with the Ford Motor Company. Card 1 1 2 3 4 5 6 7 8 Variable DT/CYCLE WEIGHT OUTPUT Type F F Default none none I 0 VARIABLE DESCRIPTION DT/CYCLE Flag for output option (time interval or cycle number). DT/CYCLE.LT.0: The absolute value is the time interval between outputs. DT/CYCLE.GT.0: Cycle numbers between outputs. WEIGHT Coefficient α in equation below. OUTPUT Output flag. When OUTPUT is set to 1, information such as integration point, element ID, time, strain ratio β, major and minor strains will be output to the “.o” file (a scratch file from batch queue run). Remarks: The incremental change of in-plane major and minor strains are smoothed according to the following formula: ∆𝜖1(𝑛−1) ∗ (1 − 𝛼) + 𝑑𝜖1(𝑛) ∗ 𝛼 ∆𝜖2(𝑛−1) ∗ (1 − 𝛼) + 𝑑𝜖2(𝑛) ∗ 𝛼 where, 𝑑𝜖1(𝑛) and 𝑑𝜖2(𝑛) are incremental changes of 𝜖1 and 𝜖2 in the current time step n, ∆𝜖1(𝑛−1) and ∆𝜖2(𝑛−1) are incremental changes of 𝜖1 and 𝜖2 in the previous time step n- 1. The weighting coefficient 𝛼 regulates the smoothness of the incremental changes in 𝜖1 and 𝜖2. Strain ratio 𝛽 results from smoothed incremental major and minor strains and stored in history variable #2 along with additional information in “.o” file if running in a batch queueing system, or directly dumped onto the screen if running in an interactive window. 𝛽 = ∆𝜖2(𝑛−1) ∗ (1 − 𝛼) + 𝑑𝜖2(𝑛) ∗ 𝛼 ∆𝜖1(𝑛−1) ∗ (1 − 𝛼) + 𝑑𝜖1(𝑛) ∗ 𝛼 The upper limit of 𝛽 is set at 1.0 while the lower limit is: where 𝑟 ̅ is the anisotropic parameter: − 𝑟 ̅ 1 + 𝑟 ̅ 𝑟 ̅ = 𝑟0 + 2𝑟45 + 𝑟90 where 𝑟0, 𝑟45 and 𝑟90 are Lankford parameter in the rolling, diagonal and transverse direction, respectively. The keyword usage is shown in the following partial input deck, where *MAT_3- PARAMETER_BARLAT_NLP is used. Note NEIPS is set at 3 for output of 3 history variables that include formability index (F.I.), strain ratio 𝛽 and effective plastic strain 𝜀̅. *KEYWORD *INCLUDE_TRIM sim_trimming.dynain ⋮ *DATABASE_EXTENT_BINARY $ NEIPH NEIPS MAXINT STRFLG SIGFLG EPSFLG RLTFLG ENGFLG 3 &nip 1 ⋮ *PARAMETER_EXPRESSION R d3plot endtime/1000.0 R nt -1.0*d3plot ... $---+----1----+----2----+----3----+----4----+----5----+----6----+----7----+----8 *CONTROL_FORMING_TOLERANC $ DT/CYCLE WEIGHT OUTPUT &nt 0.15 1 *MAT_3-PARAMETER_BARLAT_NLP $---+----1----+----2----+----3----+----4----+----5----+----6----+----7----+----8 $ MID RO E PR HR 13 7.8E-09 2.07E+05 0.30 3.000 $ M R00 R45 R90 LCID 6.000 1.200 1.450 1.090 99 $ AOPT C P VLCID NLP 2.000 200 $ A1 A2 A3 1.000 0.000 0.000 $ V1 V2 V3 D1 D2 D3 0.000 1.000 0.000 *DEFINE_CURVE 200 $FORM LIMIT DIAGRAM -0.7000 0.8309 -0.4500 0.6805 -0.2500 0.5081 0.0000 0.2479 0.2000 0.3487 0.4000 0.3845 *DEFINE_CURVE 99 0.000000000E+00 0.166100006E+03 0.579999993E-02 0.189110001E+03 0.124000004E-01 0.204789993E+03 0.190999992E-01 0.218520004E+03 0.255999994E-01 0.230580002E+03 ⋮ ⋮ 0.100000000E+01 0.512053406E+03 ... *END As shown in Figure 12-59, beta smoothed using smoothing algorithm is much better than unsmoothed one. Most importantly, a plot of strain path (Figure 12-60) in the traditional FLD space (𝜖1 vs. 𝜖2) confirms the terminal beta is approximately 0.9, which is much closer to the smoothed beta value (Figure 12-59) at the end of the simulation. Output items Columns IP # Element ID Time β 𝜖1 𝜖2 1st to 8th 9th to18th 19th to 29th 30th to 40th 41th to 51th 52th to 62th Table 12-2. “.o” file output information and positions. Note only the mid-IP information are output. Revision Information: Revision history information is listed below. Output information in “.o” file currently applies to SMP and 1 CPU MPP only. 1)LS-DYNA Revision 84159: β smoothing is enabled for *MAT_036. 2)Revision 110928: β smoothing is enabled for *MAT_037. 1.2 0.8 0.4 0.0 -0.4 0.0 Unsmoothed beta Smoothed beta 0.005 0.010 0.015 0.020 Time (seconds) Figure 12-59. Effect of smoothing on strain ration β. Terminal trendline y=1.11x+0.0651, β=0.9 0.14 0.12 0.10 0.08 0.06 0.04 0.02 0.00 0.00 0.02 0.04 0.06 0.08 0.10 0.12 0.14 Minor true strain Figure 12-60. Strain path and terminal strain ratio β value. *CONTROL_FORMING_TRAVEL Purpose: This keyword allows user to define tool travel for each phase in a stamping process simulation. The entire simulation process can be divided into multiple phases corresponding to the steps of an actual metal forming process. This keyword is to be used for tools that are pre-positioned above the sheet blank (or below the blank) and ready for forming. For tools that are pre-positioned at their home positions, *CON- TROL_FORMING_TRAVEL should be used. This keyword is used together with *CONTROL_FORMING_USER. NOTE: This option has been deprecated in favor of *CON- TROL_FORMING_AUTOPOSITION_PARAME- TER). Define Travel Cards. Repeat Card as many times as needed to define travels in multiple phases. The next “*” card terminates the input. Card 1 1 2 3 4 5 6 7 8 Variable PID VID TRAVEL TARGET GAP PHASE FOLLOW Type I I F I F I I Default none none none none 1.0t none none VARIABLE DESCRIPTION PID VID TRAVEL TARGET GAP Part ID of a stamping tool, as defined in *PART. Vector ID defining the direction of travel for the tool defined by the PID. The distance in which the tool will be traveled to complete forming in the direction specified by the VID. If TRAVEL is defined, it is unnecessary to define TARGET. Target tool PID, as defined in *PART. The tool (defined by PID) will be traveled to where the TARGET tool is to complete forming. The minimum distance between the tool (PID) and TARGET tool at the home position (forming complete). The GAP is by default the sheet blank thickness “t”. DESCRIPTION Phase number, starting sequentially from 1. For example, phase 1 is the binder closing, and phase 2 is the drawing operation. Part ID of a stamping tool to be followed by the tool (PID). When this variable is defined, the distance between the tool (PID) and part ID defined by FOLLOW, will remain constant during the phase. VARIABLE PHASE FOLLOW Remarks: FOLLOW can be used to reduce total simulation time. For example, in a toggle draw, the upper punch travels together with the upper binder during binder closing phase, thus reducing the upper travel distance during the draw, shortening the overall termination time. An example is provided in manual pages under *CONTROL_FORMING_USER. *CONTROL_FORMING_TRIM_MERGE Purpose: This feature allows for automatic close of any open trim loop curve for a successful trimming simulation. Previously, sheet metal trimming would fail if a trim curve does not form a closed loop. This keyword is used together with *DEFINE_- CURVE_TRIM, *ELEMENT_TRIM, *DEFINE_VECTOR, *CONTROL_ADAPTIVE_- CURVE, *CONTROL_CHECK_SHELL, and applies to shell elements only. Card 1 1 2 3 4 5 6 7 8 Variable IMERGE GAPM Type Default I 1 F 0.0 VARIABLE DESCRIPTION IMERGE Activation flag. Set to ‘1’ (default) to activate this feature. GAPM Gap distance between two open ends of a trim loop curve in the model. If the gap is smaller than GAPM, the two open ends of a trim curve will be closed automatically. Remarks: 1. If multiple open trim loop curves exist, GAPM should be set to a value larger than any of the gap distances of any trim curves in the trim model. 2. An example provided below shows that for both 3D (#90905) and 2D trim curve (#90907), each with an open gap of 2.3 and 2.38mm, respectively. An automatic merge operation is being performed with the GAPM set at 2.39 mm. Since this set value is larger than both gaps in the model, trimming will automatically close the gap for both curves and to form two closed-loop curves for a success- ful trim. In Figure 12-61, two different 2D trimming results are illustrated with GAPM of 2.39 (successful) as well as 2.37 (fail). *KEYWORD *INCLUDE_TRIM drawn2.dynain ⋮ *CONTROL_ADAPTIVE_CURVE $ IDSET ITYPE N SMIN &blksid 2 3 0.6 GAP=2.38 mm Trim vector 2D trim with GAPM=2.39 Trim loop curve GAP=2.38 mm 2D trim with GAPM=2.37 Figure 12-61. A 2D trimming with different GAPM values. *CONTROL_CHECK_SHELL $ PSID IFAUTO CONVEX ADPT ARATIO ANGLE SMIN &blksid1 1 1 1 0.250000150.000000 0.000000 *DEFINE_CURVE_TRIM_3D $# tcid tctype tflg tdir tctol toln nseed1 nseed2 90907 2 1 0 1.250000 2.500000 0 0 sim_trimline_03.igs *DEFINE_CURVE_TRIM_NEW $# tcid tctype tflg tdir tctol toln nseed1 nseed2 90905 2 0 2 1.250000 1.000000 0 0 $# filename sim_trimline_02.igs *DEFINE_VECTOR_TITLE vector for Trim curve 90905 $# vid xt yt zt xh yh zh cid 2 0.000 0.000 0.000 -0.170000 0.950000 -0.260000 0 *ELEMENT_TRIM &blksid *DEFINE_TRIM_SEED_POINT_COORDINATES $ NSEED,X1,Y1,Z1,X2,Y2,Z2 1,&seedx,&seedy,&seedz $---+----1----+----2----+----3----+----4----+----5----+----6----+----7----+--- -8 *CONTROL_FORMING_TRIM_MERGE $ IMERGE GAPM 1 2.39 $ Note that the 3D trim curve has a gap of 2.3 and the 2D trim curve has a gap of 2.38 *END 3. This feature is available starting in LS-DYNA Revision 84098. *CONTROL_FORMING_TRIMMING Purpose: Define a part subset to be trimmed by *DEFINE_CURVE_TRIM. This feature is intended for metal forming simulation. Currently trimming is enabled on 2D and 3D trimming of shell elements, 3D solid element, adaptive sandwiched parts (one layer of solid elements with top and bottom layers of shell elements), non-adaptive sandwiched parts (multiple layers of solid elements with top and bottom layers of shell elements), and 2-D trimming of thick shell elements (TSHELL). Note it is not applicable to axisymmetric solids or 2D plane strain/stress elements. For details, see *DEFINE_- CURVE_TRIM. NOTE: Before revision 87566 this card was called ELE- MENT_TRIM. Card 1 1 2 3 4 5 6 7 8 Variable PSID ITYP Type I Default none I 0 VARIABLE DESCRIPTION Part set ID for trimming, see *SET_PART. Activation flag for sandwiched parts (laminates) trimming: ITYP.EQ.0: Trimming for solid elements. ITYP.EQ.1: Trimming for laminates. PSID ITYP Remarks: This keyword is used together with *DEFINE_CURVE_TRIM to trim the parts defined in PSID at time zero, i.e., before any stamping process simulation begins. Elements in the part set will be automatically trimmed in the defined direction if they intersect the trim curves. See examples in keyword section *DEFINE_CURVE_TRIM. *CONTROL_FORMING_TRIMMING 1. Revision 87566: *ELEMENT_TRIM was changed to the current name *CON- TROL_FORMING_TRIMING. 2. Revision 95745: *CONTROL_FORMING_TRIMING was changed to *CON- TROL_FORMING_TRIMMING. 3. Revision 92088: 2-D trimming of solid elements is implemented. 4. Revision 92289: 2-D and 3-D trimming of laminates (ITYP) is added. 5. Revision 93467: 3-D trimming of solid elements is added. 6. Latter Revisions may incorporate more improvements and are suggested to be used for trimming. *CONTROL_FORMING_UNFLANGING_{OPTION} Available options include: <BLANK> OUTPUT Purpose: The keyword unfolds flanges of a deformable blank onto a rigid tooling mesh using an implicit statics solver. This is typically used in trim line unfolding during a stamping die development process. The option OUTPUT must be used together with *CONTROL_FORMING_UNFLANGING to get the modified trim curves. Other keywords related to blank size development are, *CONTROL_FORMING_ONESTEP, and *INTERFACE_BLANKSIZE_DEVELOPMENT. Card 1 for no option, <BLANK>: Card 1 1 2 3 4 5 6 7 8 Variable NOPTION DVID NUNBEND STFBEND STFCNT IFLIMIT DIST ILINEAR Type I I I F F I F Default none N/A none none none none none I 2 Card 2 for no option, <BLANK>: Card 1 1 2 3 4 5 6 7 8 Variable NB1 NB2 NB3 CHARLEN NDOUTER Type I I I F I Default none none none 150.0 none *CONTROL_FORMING_UNFLANGING Card 1 1 2 3 4 5 6 7 8 Variable THMX THMN EPSMX Type I I I Default 1020 0.0 1020 VARIABLE DESCRIPTION NOPTION Flag to turn on an unfolding simulation: EQ.1: Activate the unfolding simulation program. DVID This variable is currently not being used. NUNBEND Estimated number of unbending, ranging from 10 to 100. STFBEND Unflanging stiffness, ranging from 0.1 to 10.0. STFCNT Normal stiffness, ranging from 0.1 to 10.0. IFLIMIT DIST Iteration limit for the first phase of unfolding, typically ranging from 11 to 400. Distance tolerance for auto-SPC along flange root. DIST (Figure 12-63) is usually slightly more than ½ of the flange thickness. This field must be left blank for ILINEAR = 2. Also, nodes along the root can be directly positioned on the rigid body surface (addendum), leaving a DIST of zero (Figure 12-63). ILINEAR Unfolding algorithm selection flag: EQ.0: Nonlinear unfolding. EQ.1: Linear unfolding. EQ.2: A hybrid unfolding method (Revision 87100 and later). The curved 3D meshes of the flange will first be mapped onto the tooling surface to be used as a starting porting for nonlinear iterations; unfolding completes when force balance is reached. (recommended). VARIABLE NB1 NB2 NB3 CHARLEN NDOUTER THMX DESCRIPTION The start node ID (Figure 12-64) on a flange root boundary (fixed end of the flange, see Figures 12-63 and 12-64). For closed-loop flange root boundary, only this parameter needs to be defined; for open-loop flange root boundary, define this parameter as well as NB2 and NB3. The solver will automatically identify and automatically impose the necessary boundary constraints on all the nodes along the entire three-dimensional flange root boundary. The ID of a node in the middle of the flange root boundary, see Figure 12-64. Define this parameter for open-loop flange root boundary only. The end node ID on a flange root boundary. Define this parameter for open-loop flange root boundary only. The “path” formed by NB1, NB2 and NB3 can be in any direction, meaning NB1 and NB3 (Figure 12-64) can be interchangeable. Maximum flange height (Figure 12-64) to limit the search region for the boundary nodes along the flange root. This value should be set bigger than the longest width (height) of the flange; and it is needed in some cases. This parameter is now automatically calculated as of Revision 92860. A node ID on the outer flange (free end of the flange) boundary. This node helps search of nodes along the flange root, especially when holes are present in the flange area, see Figure 12-64. Maximum thickness beyond which elements are deleted; this is useful in removing wrinkling areas of the flange (shrink flange). Modified, unfolded flange outlines based on this parameter are stored in a file called “trimcurve_upd.k”, written using the *DE- FINE_CURVE_TRIM_3D; keyword. The modified flanges (before unfolding) are in a keyword file called “mdfiedflangedpart.k”; and the unmodified flange (unfolded) is in “trimcurve_nmd.k”, also written using keyword *DEFINE_CURVE_TRIM_3D. See the example in Figure 12-64 for an explanation. Currently the modified flange and curves are not smooth, which will be improved in the future. To convert between *DEFINE_CURVE_- TRIM_3D and IGES format, refer to Figures in *INTERFACE_- BLANKSIZE. THMN *CONTROL_FORMING_UNFLANGING DESCRIPTION Minimum thickness below which elements are deleted; this is useful in removing overly thinned areas of the flange (stretch flange). Updated flange information based on this parameter is stored in files listed above. EPSMX Maximum effective plastic strain beyond which elements are deleted; this is useful in removing flange areas with high effective plastic strains (stretch flange). Updated flange information based on this parameter is stored in files listed above. Introduction: Unfolding of flanges is one of the first steps in a stamping die development process. Immediately after tipping, binder and addendums are built for unfolding of flanges. According to process considerations (trim conditions, draw depth, and material utilization, etc.), the addendums are built either in parallel or perpendicular to the draw die axis, tangentially off the main surface off the breakline , or any combinations of the three scenarios. Trim lines are developed by unfolding the flanges in finished (hemmed or flanged) position onto these addendums. Addendum length in some areas may have to be adjusted to accommodate the unfolded trim lines. Trim line development is very critical in hard tool development. Inaccurate trim lines lead to trim die rework, result in many hours of re-welding, re-machining and re-spotting of trim die components. Input and output: The inputs for the keyword are: 1. blank or flanges in the finished configuration, and, 2. the draw die surface in mesh. Meshes for flanges should of a quality similar to the blank mesh one would build for a forming simulation. In LS-PrePost 4.0, this kind of mesh can be created using Mesh → Automesh → Size. Element formulation 16 with NIP set to 5 is recommended for the blank. The output results, in terms of unfolding steps and final unfolded flanges, are stored in the d3plot files. LS-PrePost 4.0 function of Curve → Spline → From Mesh → By part can be used to create unfolded flange/trim curves from the unfolded flanges. Since the program uses an implicit statics solver, the double precision version of LS-DYNA must be used. Other modeling guidelines: 1. All addendum and flanges need to be oriented as if they are in a draw position, with the drawing axis parallel to the global Z-axis; specifically the flanges need to be on top of the addendum, as noted in Figures 12-62, 12-63 and 12-64. 2. Normals of the to-be-unfolded flange side and tool surface side must be consistent and must face against each other when the flange is unfolded, see Figure 12-64. 3. Holes in the blank are allowed only for ILINEAR = 2. 4. Adaptive re-meshing is not supported. 5. To-be-unfolded flange and tool meshes must not share the same nodes. This can be easily done using the mesh detaching feature under EleTol → DetEle in LS-PrePost. 6. Meshes of the flange part and rigid tool can slightly overlap each other, but large amounts of overlap (area of flange already on addendum surface) is not allowed. In LS-PrePost the EleTol → PtTrim feature can trim off the overlapped flange portion. The curves used for the trimming can be obtained from the flange tangent curves on the addendum (which has a more regulated mesh pattern) using LS-PrePost’s Curve → Spline → Method From Mesh → By Edge → Prop feature with appropriate angle definition. Furthermore, any holes are not allowed in the overlapping area. 7. *CONTACT_FORMING_ONE_WAY_SURFACE_TO_SURFACE should be used for the contact between the blank and tool. Negative tool offsets on the *CONTACT_… keyword is not supported. 8. The rigid tool (total fixed in *MAT_020) must be larger than the unfolded flanges, especially along symmetric lines. This may be obvious, nevertheless it is sometimes overlooked. 9. Nodes along the flange root are automatically fixed by defining NB1, NB2 and NB3, as shown in Figure 12-64. 10. No “zigzag” along the flange root boundary, meaning that the boundary along the flange root must be smooth. This restriction is removed as of Revision 92727. 11. Symmetric boundary conditions are supported. 12. Thickness and effective plastic strain are stored in a file “unflanginfo.out”, which can be plotted in LS-PrePost 4.0, see Figure 12-64. *CONTROL_FORMING_UNFLANGING A partial input deck is provided below for flange unfolding of a fender outer, modified from the original NCAC Taurus model. Shown in Figure 12-62 are the progressions of the unfolding process, where the finished flanges are to be unfolded onto the addendum (rigid body). A section view of the same unfolding before and after is found in Figure 12-63. ILINEAR is set at 2 while DIST is left blank. Total numbers of elements are 1251 on the blank and 6600 on the tooling. It took less than 3 minutes on an 8 CPU (SMP) machine. Note that additional keywords, such as *CONTROL_IMPLICIT_- FORMING, etc. are used. Termination criterion is set using the variable DELTAU in *CONTROL_IMPLICIT_TERMINATION. Termination is reached when the relative displacement ratio criterion is met, as indicated in the messag file. Termination time of 10.0 (steps) is sufficient for most cases, but may need to be extended in some cases to satisfy the DELTAU in some cases. $---+----1----+----2----+----3----+----4----+----5----+----6----+----7----+----8 *KEYWORD *INCLUDE toolblankmesh.k *CONTROL_FORMING_UNFLANGING $ NOPTION DVID NUNBEND STFBEND STFCNT IFLIMIT DIST ILINEAR 1 100 0.2 15.0 400 2 $ NB1 NB2 NB3 CHARLEN NDOUTER 321 451 322 60.0 6245 *CONTROL_IMPLICIT_FORMING 1 *CONTROL_IMPLICIT_TERMINATION $ DELTAU $ set between 0.0005~0.001 0.0005 *CONTROL_IMPLICIT_GENERAL $ IMFLAG DT0 1 .1000 *CONTROL_IMPLICIT_SOLUTION $ NSLOLVR ILIMIT MAXREF DCTOL ECTOL RCTOL LSTOL 2 2 1100 0.100 1.e20 1.e20 $ dnorm divflag inistif 0 2 0 1 1 *PARAMETER R ENDTIME 10.0 I elform 16 I nip 5 R bthick 1.0 *PARAMETER_EXPRESSION R D3PLOTS ENDTIME/60.0 *CONTROL_TERMINATION &ENDTIME *DATABASE_BINARY_D3PLOT &D3PLOTS *CONTROL_RIGID... *CONTROL_HOURGLASS... *CONTROL_BULK_VISCOSITY... *CONTROL_SHELL... *CONTROL_CONTACT $ SLSFAC RWPNAL ISLCHK SHLTHK PENOPT THKCHG ORIEN 0.01 0.0 2 1 4 0 4 $ USRSTR USRFAC NSBCS INTERM XPENE SSTHK ECDT TIEDPRJ 0 0 10 0 2.0 0 *CONTROL_ENERGY... *CONTROL_ACCURACY... *DATABASE_EXTENT_BINARY... *SECTION_SHELL_TITLE BLANK/FLANGE thickness and elform/nip specs. &blksec &elform 0.833 &nip 1.0 &bthick,&bthick,&bthick,&bthick *PART... *MAT_TRANSVERSELY_ANISOTROPIC_ELASTIC_PLASTIC... *MAT_RIGID... *CONTACT_FORMING_ONE_WAY_SURFACE_TO_SURFACE $ SSID MSID SSTYP MSTYP SBOXID MBOXID SPR MPR &blkpid &diepid 3 3 $ FS FD DC VC VDC PENCHK BT DT 0.125 0.0 0.0 0.0 20.0 0 0.0 1.000E+20 $ SFS SFM SST MST SFST SFMT FSF VSF 1.0 1.0 0.0 $ SOFT SOFSCL LCIDAB MAXPAR PENTOL DEPTH BSORT FRCFRQ 0 $ PENMAX THKOPT SHLTHK SNLOG ISYM I2D3D SLDTHK SLDSTF $ IGAP IGNORE DPRFAC DTSTIF FLANGL 2 *END In Figure 12-64 (top), with THMN set at 0.4mm, the stretch flange area of the corner, which has thickness less than 0.4mm, is removed; and the modified flange outlines are created accordingly (bottom). The partial input used is listed below. *CONTROL_FORMING_UNFLANGING $ NOPTION DVID NUNBEND STFBEND STFCNT IFLIMIT DIST ILINEAR 1 100 0.2 15.0 400 2 $ NB1 NB2 NB3 CHARLEN NDOUTER 321 451 322 60.0 6245 *CONTROL_FORMING_UNFLANGING $ THMX THMN EPSMX 0.4 Revision information: The feature is available in double precision SMP, and starting in LS-DYNA Revision 73190. Revision information is listed below for various parameters and features: 1. ILINEAR = 2: Revision 87100. 2. NDOUTER: Revision 87318. 3. CHARLEN: Revision 87210. 4. NB1, NB2, NB3: Revision 87100. 5. Option OUTPUT: Revision 86943. 6. Holes allowed: Revision 87167. 7. File “mdfiedflangedpart”: Revision 87105. 8. Symmetric boundary condition: Revision 88359. 9. CHARLEN automatically calculated: Revision 92860. 10. “Zigzag” flange root boundary allowed: Revision 92727. Finished flanges 30% unfolded Flanges must be on top of the addendum in the draw position Addendum 60% unfolded Unfolded flanges 100% unfolded Figure 12-62. Flange unfolding progression of a fender outer (original model courtesy of NCAC at George Washington University). Addendum Finished (incoming) flanges Unfolded flanges Flange root (fixed end) Free end of the flange Flanges must be on top of the addendum in the draw position DIST Figure 12-63. A section view showing flange unfolding before and after. Thickness contour min=0.2257 max=0.8533 Thickness (mm) Holes are allowed Thickness in the dark blue area less than 0.4mm, at which THMN is set. Flange normals Addendum normals 0.85 0.79 0.73 0.67 0.60 0.54 0.48 0.41 0.35 0.29 0.23 Addendum surface Flange before unfolding Unfolded flange. Thickness and effective plastic strain contour are stored in a file "unflanginfo.out" NB3 Flange must be on top of the addendum in the draw position CHARLEN NDOUTER NB2 Flange root boundary (fixed) NB1 - define this only for a closed-loop boundary; define all three (NB1, NB2, NB3) for an open-loop boundary. Original flange is modified based on THMN=0.4 and the mesh is stored in a file "mdfiedflangedpart.k". Boundary curves can be created using LSPP4.0 under Curve/Spline/From mesh/by part. Modified boundary curves on unfolded flange are stored in a file "trimcurve_upd.k"; original boundary curves (without the corner cutout) is in "trimcurve_nmd.k". Figure 12-64. Unfolding details and output files *CONTROL_FORMING_USER Purpose: This keyword, along with *CONTROL_FORMING_POSITION, or *CON- TROL_FORMING_TRAVEL, allow user to set up a stamping process simulation. From this card various model parameters may be specified: • material properties, • material model, • tooling kinematics, • mesh adaptivity • D3PLOT generation NOTE: This option has been deprecated in favor of *CON- TROL_FORMING_AUTOPOSITION_PARAME- TER). Card 1 1 2 3 4 5 6 7 8 Variable BLANK TYPE THICK R00 R45 R90 AL/FE UNIT Type I Default none Card 2 1 Variable LCSS Type I I 0 2 K F F F F F none 1.0 R00 R00 3 N F 4 E F 5 6 DENSITY PR F F A F 7 FS F I 1 8 MTYPE I Default none none none none none none 0.1 37 Card 3 1 2 3 4 5 6 7 8 Variable PATERN VMAX AMAX LVLADA SIZEADA ADATIMS D3PLT GAP Type Default I 1 F F 1000.0 500000. I 0 F 0 I 0 I F 10 1.1t VARIABLE DESCRIPTION BLANK PID of a sheet blank, as in *PART. TYPE Flag of part or part set ID for the blank: EQ.0: Part ID. EQ.1: Part set ID. THICK R00, R45, R90 AL/FE UNIT LCSS Thickness of the blank. This variable is ignored if the thickness is already defined in *SECTION_SHELL. Material anisotropic parameters. For transverse anisotropy the R value is set to the average value of R00, R45, and R90. This parameter is used to define the Young’s Modulus, E, and density, ρ, for the sheet blank. If this variable is defined, E and ρ will be found by using the proper unit, as listed in Table 8.1, under *CONTROL_FORMING_TEMPLATE. EQ.A: the blank is aluminum EQ.F: the blank is steel (default) Units adopted in this simulation. Define a number between 1 and 10. Table 8.1 is used to determine the value for UNIT. This unit is used to obtain proper values for punch velocity, acceleration, time step, and physical and material properties. If the material for the blank has not been defined, this curve will be used to define the stress-strain relation. Otherwise, this variable is ignored. PREBD “Pull-over” distance for the upper and lower binders after closing in a 4-piece stretch draw, as shown in Figure 12-57. VARIABLE DESCRIPTION K N E Strength coefficient for exponential hardening (𝜎̅̅̅̅̅ = 𝑘𝜀̅ 𝑛). If LCSS is defined, or if a blank material is defined with *MAT_036 or *MAT_037, this variable is ignored. Exponent for exponential hardening (𝜎̅̅̅̅̅ = 𝑘𝜀̅ 𝑛). If LCSS is defined, or if a blank material is defined with *MAT_036 or *MAT_037, this variable is ignored. Young’s Modulus. If AL/FE is user defined, E is unnecessary. DENSITY Material density of the blank. If AL/FE is defined, this variable is unnecessary. PR FS MTYP Poisson’s ratio. If AL/FE is user defined, this variable is unnecessary. Coulomb friction coefficient. If contact is defined with *CON- TACT_FORMING_..., this variable is ignored. Material model identification number, for example, 36 for *MAT_036 and 37 for *MAT_037. Currently only material models 36 and 37 are supported. PATERN Velocity profile of the moving tool. If the velocity and the profile are defined by *BOUNDARY_PRESCRIBED_MOTION_RIGID, and *DEFINE_CURVE, this variable is ignored. EQ.1: Ramped velocity profile. EQ.2: Smooth velocity curve. VMAX The maximum allowable tool travel velocity. AMAX The maximum allowable tool acceleration. LVLADA Maximum mesh adaptive level. SIZEADA Minimum element size permitted during mesh adaptivity. ADATIMS Total number of adaptive steps during the simulation. D3PLT The total number of output states in the D3PLOT database. GAP Minimum gap between two closing tools at home position, in the travel direction of the moving tool. This variable will be used for *CONTROL_FORMING_POSITION. Keyword examples: A partial keyword example provided below is for tools in their home positions in a simple 2-piece crash forming die. A steel sheet blank PID 1, is assigned with a thickness of 0.76mm (UNIT = 1) and *MAT_037 with anisotropic values indicated, to follow hardening curve of 90903, form in a ‘ramped’ type of velocity profile with maximum velocity of 5000mm/s and acceleration of 500000.0 mm/s2, adapt mesh 5 levels with smallest adapted element size of 0.9 for a total of 20 adaptive steps, create a total of 15 post-processing states, and to finish forming with a final gap of 1.1mm between the tools (PID3 and 5) at home position. The upper tool with PID 3 is to be moved back in Z axis to clear the interference with the blank before close toward the lower tool of target PID 5. *CONTROL_FORMING_USER $ BLANK TYPE THICK R00 R45 R90 AL/FE UNIT 1 0 0.76 1.5 1.6 1.4 F 1 $ LCSS K N E DENSITY PR FS MTYPE 90903 37 $ PATTERN VMAX AMAX LVLADA SIZEADA ADATIMS D3PLT GAP 1 5000.0 500000.0 5 0.9 20.0 15.0 1.1 $---+----1----+----2----+----3----+----4----+----5----+----6----+----7----+----8 *CONTROL_FORMING_POSITION $ This is for tools in home position. $ PID PREMOVE TARGET 3 5 The following partial keyword example is for tools already positioned in relationship to the blank and ready to close. All assigned properties for the blank remain the same. Here the upper tool PID3 is not going to be moved back, but instead it will move forward to close with the lower tool of target PID 5 in the direction specified by the vector ID 999. *CONTROL_FORMING_USER 1 0 1.0 1.5 1.6 1.4 F 1 90903 37 1 5000.0 500000.0 5 0.9 20.0 15.0 1.1 *CONTROL_FORMING_TRAVEL $ PID VID TRAVEL TARGET GAP PHASE FOLLOW 3 999 5 1.1 1 Revision information: This keyword is available starting in LS-DYNA Revision 48319. *CONTROL_FREQUENCY_DOMAIN Purpose: Set global control flags and parameters for frequency domain analysis. Card 1 1 2 3 4 5 6 7 8 Variable REFGEO MPN Type Default I 0 F 0.0 VARIABLE DESCRIPTION REFGEO Flag for reference geometry in acoustic eigenvalue analysis: EQ.0: use original geometry (t = 0), EQ.1: use deformed geometry at the end of transient analysis. MPN Large mass added per node, to be used in large mass method for enforced motion. Remarks: 1. For acoustic eigenvalue keyword *FREQUENCY_DOMAIN_ACOUSTIC_ FEM_EIGENVALUE), sometimes it is desired to extract the eigenvalues at the end of transient analysis, based on the deformed geometry. This is useful to study the effect of loading history on acoustic eigenvalues. In this case, one can set REFGEO = 1 to use the deformed geometry at the end of transient analysis. analysis in FRF, SSD, or random vibration analysis, one can use the large mass method to compute the response. With the large mass method, the user attach- es a large mass to the nodes under excitation. LS-DYNA converts the enforced motion excitation to nodal force on the same nodes in the same direction, to produce the desired enforced motion. MPN is the large mass attached to each node under excitation (usually it is in the range of 105-107 times of the original mass of the entire structure). User still need to apply the large mass to the nodes using the keyword *ELEMENT_MASS_{OPTION}. The large nodal force p is computed as follows, For nodal acceleration, 𝑝 = 𝑚𝐿𝑢̈ For nodal velocity, 𝑝 = 𝑖 𝜔𝑚𝐿𝑢̇ For nodal displacement, 𝑝 = − 𝜔2𝑚𝐿𝑢 where 𝜔 is the round frequency, 𝑚𝐿 is the large mass attached to each node (MPN), 𝑢̈, 𝑢̇ and 𝑢 are the enforced acceleration, velocity and displacement. *CONTROL_HOURGLASS_{OPTION} Available options include: <BLANK> 936 The “936” option switches the hourglass formulation for shells so that it is identical to that used in LS-DYNA version 936. The modification in the hourglass control from version 936 was to ensure that all components of the hourglass force vector are orthogonal to rigid body rotations. However, problems that run under version 936 sometimes lead to different results in versions 940 and later. This difference in results is primarily due to the modifications in the hourglass force vector. Versions released after 936 should be more accurate. Purpose: Redefine the default values of hourglass control type and coefficient. 3 4 5 6 7 8 Card 1 1 Variable IHQ Type I Default 2 QH F 0.1 Remarks 1,2 3,4 VARIABLE DESCRIPTION IHQ Default hourglass control type: EQ.0: see Remark 1, EQ.1: standard viscous form (may inhibit body rotation if solid element shapes are skewed), EQ.2: viscous form, Flanagan-Belytschko integration for solid elements, EQ.3: viscous form, Flanagan-Belytschko with exact volume integration for solid elements, EQ.4: stiffness form of type 2 (Flanagan-Belytschko), EQ.5: stiffness form of type 3 (Flanagan-Belytschko) for solid VARIABLE DESCRIPTION elements, EQ.6: Belytschko-Bindeman [1993] assumed strain co- rotational stiffness form for 2D and 3D solid elements, EQ.7: Linear total strain form of type 6 hourglass control. EQ.8: Activates full projection warping stiffness for shell formulations 16 and -16, and is the default for these shell formulations. A speed penalty of 25% is common for this option. EQ.9: Puso [2000] enhanced assumed strain stiffness form for 3D hexahedral elements, EQ.10: Cosserat Point Element (CPE) developed by Jabareen and Rubin [2008] for 3D hexahedral elements and Jab- areen et.al [2013] for 10-noded tetrahedral elements. See Remark 6. QH Default hourglass coefficient. Remarks: 1. Hourglass control is viscosity or stiffness that is added to quadrilateral shell elements and hexahedral solid elements that use reduced integration. It also applies to type 1 tshells. Without hourglass control, these elements would have zero energy deformation modes which could grow large and destroy the solu- tion. *CONTROL_HOURGLASS can be used to redefine the default values of the hourglass control type and coefficient. If omitted or if IHQ = 0, the default hourglass control types are as follows: a) For shells: viscous type for explicit; stiffness type for implicit. b) For solids: type 2 for explicit; type 6 for implicit. c) For tshell formulation 1: type 2. These default values are used unless HGID on *PART is used to point to *HOURGLASS data which overrides the default values for that part. For explicit analysis, shell elements can be used with viscous hourglass control, (IHQ = 1 = 2 = 3) or stiffness hourglass control (IHQ = 4 = 5). Only shell forms 16 and -16 use the warping stiffness invoked by IHQ = 8. For implicit analysis, the viscous form is unavailable. For explicit analysis, hexahedral elements can be used with any of the hourglass control types except IHQ = 8. For implicit analysis, only IHQ = 6, 7, 9, and 10 are available. If IHQ is set to a value that is invalid for some elements in a model, then the hourglass control type for those elements is automatically reset to a valid value. For explicit analysis, if IHQ = 6, 7, 9, or 10, then shell elements will be switched to type 4 except for form 16 and -16 shells that are switched to type 8. If IHQ = 8, then solid elements and shell elements that are not form 16 or -16 will be switched to type 4. For implicit analysis, if IHQ = 1-5, then solid elements will be switched to type 6, and if IHQ = 1, 2, 3, 6, 7, 9, or 10, then shell elements will switched to type 4. 2. Viscous hourglass control has been used successfully with shell elements when the response with stiffness based hourglass control was overly stiff. As models have grown more detailed and are better able to capture deformation modes, there is less need for viscous forms. To maintain back compatibility, viscous hourglass control remains the default for explicit analysis, but there may be better choices, particularly the newer forms for bricks (6, 7, 9, and 10). 3. QH is a coefficient that scales the hourglass viscosity or stiffness. With IHQ = 1 through 5 and IHQ = 8, values of QH that exceed 0.15 may cause instabilities. Hourglass types 6, 7, 9, and 10 will remain stable with larger QH and can work well with QH = 1.0 for many materials. However, for plasticity models, a smaller value such as QH = 0.1 may work better since the hourglass stiffness is based on elastic properties. 4. Hourglass types 6, 7, 9, and 10 for hexahedral elements are based on physical stabilization using an enhanced assumed strain method. When element meshes are not particularly skewed or distorted, their behavior may be very similar and all can produce accurate coarse mesh bending results for elastic material with QH = 1.0. However, form 9 gives more accurate results for distorted or skewed elements. In addition, for materials 3, 18 and 24 there is the option to use a negative value of QH. With this option, the hourglass stiffness is based on the current material properties, i.e., the plastic tangent modulus, and scaled by |QH|. 5. Hourglass type 7 is a variation on form 6. Instead of updating the hourglass forces incrementally using the current stiffness and an increment of defor- mations, the total hourglass deformation is evaluated each cycle. This ensures that elements always spring back to their initial geometry if the load is removed and the material has not undergone inelastic deformation. Hourglass type 7 is recommended for foams that employ *INITIAL_FOAM_REFERENCE_GEOM- ETRY. However the CPU time for type 7 is roughly double that for type 6, so it is only recommended when needed. 6. Hourglass type 10 for 1-point solid elements or 10-noded tetrahedron of type 16 are strucural elements based on Cosserat point theory that allows for accurate representation of elementary deformation modes (stretching, bending and torsion) for general element shapes and hyperelastic materials. To this end, the theory in Jabareen and Rubin [2008] and Jabareen et.al [2013] has been general- ized in the implementation to account for any material response. The defor- mation is separated into a homogenous and an inhomogeneous part where the former is treated by the constitutive law and the latter by a hyperelastic formu- lation that is set up to match analytical results for the deformation modes men- tioned above. Tests have shown that the element is giving more accurate results than other hexahedral elements for small deformation problems and more realistic behavior in general. *CONTROL_IMPLICIT Purpose: Set parameters for implicit calculation features. *CONTROL_IMPLICIT_AUTO *CONTROL_IMPLICIT_BUCKLE *CONTROL_IMPLICIT_CONSISTENT_MASS *CONTROL_IMPLICIT_DYNAMICS *CONTROL_IMPLICIT_EIGENVALUE *CONTROL_IMPLICIT_FORMING *CONTROL_IMPLICIT_GENERAL *CONTROL_IMPLICIT_INERTIA_RELIEF *CONTROL_IMPLICIT_JOINTS *CONTROL_IMPLICIT_MODAL_DYNAMIC *CONTROL_IMPLICIT_MODAL_DYNAMIC_DAMPING_{OPTION} *CONTROL_IMPLICIT_MODAL_DYNAMIC_MODE_{OPTION} *CONTROL_IMPLICIT_MODES_{OPTION} *CONTROL_IMPLICIT_ROTATIONAL_DYNAMICS *CONTROL_IMPLICIT_SOLUTION *CONTROL_IMPLICIT_SOLVER *CONTROL_IMPLICIT_STABILIZATION *CONTROL_IMPLICIT_STATIC_CONDENSATION *CONTROL_IMPLICIT_TERMINATION *CONTROL_IMPLICIT_AUTO_{OPTION} Available options for OPTION include: <BLANK> DYN SPR Purpose: Define parameters for automatic time step control during implicit analysis . The DYN option allows setting controls specifically for the dynamic relaxation phase. The SPR option allows setting controls specifically for the springback phase. Card 1 1 2 3 4 5 6 7 8 Variable IAUTO ITEOPT ITEWIN DTMIN DTMAX DTEXP KFAIL KCYCLE Type Default I 0 I 11 I 5 F F F DT/1000. DT×10. none VARIABLE DESCRIPTION IAUTO Automatic time step control flag EQ.0: constant time step size EQ.1: automatically adjust time step size EQ.2: automatically adjust time step size and synchronize with thermal mechanical time step. LT.0: Curve ID = (-IAUTO) gives time step size as a function of time. If specified, DTMIN and DTMAX will still be ap- plied. ITEOPT ITEWIN Optimum equilibrium iteration count per time step. See Figure 12-65. Allowable iteration window. If iteration count is within ITEWIN iterations of ITEOPT, step size will not be adjusted for the next step. ITEOPT + ITEWIN ITEOPT ITEOPT - ITEWIN No Auto-Adjust Zone Figure 12-65. Iteration Window as defined by ITEOPT and ITEWIN. Solution Time VARIABLE DTMIN DESCRIPTION Minimum allowable time step size. Simulation stops with error termination if time step falls below DTMIN. DTMAX Maximum allowable time step size. DTEXP KFAIL LT.0: curve ID = (-DTMAX) gives max step size as a function of time. Also, the step size is adjusted automatically so that the time value of each point in the curve is reached exact- ly . Time interval to run in explicit mode before returning to implicit mode. Applies only when automatic implicit-explicit switching is active (IMFLAG = 4 or 5 on *CONTROL_IMPLICIT_GENERAL). Also, see KCYCLE. EQ.0: defaults to the current implicit time step size. LT.0: curve ID = (-DTEXP) gives the time interval as a function of time. Number of failed attempts to converge implicitly for the current time step before automatically switching to explicit time integration. Applies only when automatic implicit-explicit switching is active. The default is one attempt. If IAUTO = 0, any input value is reset to unity. DT0 DTMAX > 0 DTMAX > 0 time step value DTMIN DTMIN Time Figure 12-66. The implicit time step size changes continuously as a function of convergence within the bounds set by DTMIN and DTMAX VARIABLE KCYCLE Remarks: VARIABLE IAUTO ITEOPT DESCRIPTION Number of explicit cycles to run in explicit mode before returning to the implicit mode. The actual time interval that is used will be the maximum between DTEXP and KCYCLE*(latest estimate of the explicit time step size). REMARK The default for IAUTO depends on the analysis type. For “springback” analysis, automatic time step control and artificial stabilization are activated by default. With IAUTO = 1 or 2, the time step size is adjusted if convergence is reached in a number of iterations that falls outside the specified “iteration window”, increasing after “easy” steps, and decreasing ITEOPT defines the after “difficult” but successful steps. midpoint of the iteration window. A value of ITEOPT = 30 or more can be more efficient for highly nonlinear simulations by allowing more iterations in each step, hence fewer total steps. ITEWIN The step size is not adjusted if the iteration count falls within ITEWIN of ITEOPT. Large values of ITEWIN make the controller more tolerant of variations in iteration count. 2.0 1.0 0.0 -1.0 DTMAX active from previous key point to current key point A key point is automatically generated at the termination time Problem Time end negative value ⇒ d3plot output suppressed = Load curve points (DTMAX < 0), also key points = LS-DYNA generated key point Figure 12-67. DTMAX < 0. The maximum time step is set by a load curve of LCID = −DTMAX interpolated using piecewise constants. The abscissa values of the load curve determine the set of key points. The absolute value of the ordinate values set the maximum time step size. Key points are special time values for which the integrator will adjust the time step so as to reach exactly. For each key point with a positive function value, LS-DYNA will write the state to the binary database. VARIABLE DTMAX DTEXP REMARK To strike a particular simulation time exactly, create a key point curve (Figure 12-67) and enter DTMAX = -(curve ID). This is useful to guarantee that important simulation times, such as when peak load values occur, are reached exactly. When the automatic implicit-explicit switching option is activated (IMFLAG = 4 or 5 on *CONTROL_IMPLICIT_GENERAL), the solution method will begin as implicit, and if convergence of the equilibrium iterations fails, automatically switch to explicit for a time interval of DTEXP. A small value of DTEXP should be chosen so that significant dynamic effects do not develop during the explicit phase, since these can make recovery of nonlinear equilibrium difficult during the next implicit time step. A reasonable starting value of DTEXP may equal several hundred VARIABLE REMARK explicit time steps. *CONTROL_IMPLICIT_BUCKLE Purpose: Activate implicit buckling analysis when termination time is reached . Optionally, buckling analyses are performed at intermittent times. Card 1 1 2 3 4 5 6 7 8 Variable NMODE BCKMTH Type I I Default 0 see below VARIABLE DESCRIPTION NMODE Number of buckling modes to compute EQ.0: none (DEFAULT) GT.0: compute n lowest buckling modes LT.0: curve ID = (-NEIG) used for intermittent buckling analysis BCKMTH Method used to extract buckling modes EQ.1: Use Block Shift and Invert Lanczos. Default of all problems not using *CONTROL_IMPLICIT_INERTIA_- RELIEF. EQ.2: Use Power Method. Only valid option for problems using *CONTROL_IMPLICIT_INERTIA_RELIEF. Op- tional for other problems. See Remarks. Remarks: Buckling analysis is performed at the end of a static implicit simulation or at specified times during the simulation. The simulation may be linear or nonlinear but must be implicit. After loads have been applied to the model, the buckling eigenproblem is solved: [𝐊𝑀 + 𝜆𝐊𝐺]{𝑢} = 0 where 𝐊𝑀 is the material tangent stiffness matrix, and the geometric or initial stress stiffness matrix 𝐊𝐺 is a function of internal stress in the model. The lowest n eigenvalues and eigenvectors are computed. The eigenvalues, written to text file “eigout”, represent multipliers to the applied loads which give buckling loads. The eigenvectors, written to binary database “d3eigv”, represent buckling mode shapes. View and animate these modes using LS-PrePost. When NMODE > 0, eigenvalues will be computed at the termination time and LS-DYNA will terminate. When NMODE < 0, an intermittent buckling analysis will be performed. This is a transient simulation during which loads are applied, with buckling modes computed periodically during the simulation. Changes in geometry, stress, material, and contact conditions will affect the buckling modes. The transient simulation must be implicit. The curve ID = -NMODE indicates when to extract the buckling modes, and how many to extract. Define one curve point at each desired extraction time, with a function value equal to the number of buckling modes desired at that time. A d3plot database will be produced for the transient solution results. Consecutively numbered d3eigv and eigout databases will be produced for each intermittent extraction. The extraction time is indicated in each database’s analysis title. The buckling modes can be computed using either Block Shift and Invert Lanczos or the Power Method. It is strongly recommended that the Block Shift and Invert Lanczos method is used as it is a more powerful and robust algorithm. For problems using *CONTROL_IMPLICIT_INERTIA_RELIEF the Power Method must be used and any input value for BCKMTH will be overridden with the required value of 2. There may be some problems, which are not using *CONTROL_IMPLICIT_INERTIA_RELIEF, where the Power Method may be more efficient than Block Shift and Invert Lanczos. But the Power Method is not as robust and reliable as Lanczos and results should be verified. Furthermore convergence of the Power Method is better for buckling problems where the expected buckling mode is close to one in magnitude and the dominant mode is separated from the secondary modes. The number of modes extracted via the Power Method should be kept in the range of 1 to 5. The geometric stiffness terms needed for buckling analysis will be automatically computed when the buckling analysis time is reached, regardless of the value of the geometric stiffness flag IGS on *CONTROL_IMPLICIT_GENERAL. A double precision executable should be used for best accuracy in buckling analysis. Parameters CENTER, LFLAG, LFTEND, RFLAG, RHTEND and SHFSCL from *CON- TROL_IMPLICIT_EIGENVALUE are applicable to buckling analysis. For buckling analysis CENTER, LFTEND, RHTEND and SHFSCL are in units of the eigenvalue spectrum. *CONTROL_IMPLICIT_CONSISTENT_MASS Purpose: Use the consistent mass matrix in implicit dynamics and eigenvalue solutions. Card 1 1 2 3 4 5 6 7 8 Variable IFLAG Type Default I 0 VARIABLE DESCRIPTION IFLAG Consistent mass matrix flag EQ.0: Use the standard lumped mass formulation (DEFAULT) EQ.1: Use the consistent mass matrix. Remarks: The consistent mass matrix formulation is currently available for the three and four node shell elements, solid elements types 1, 2, 10, 15, 16, and 18 , and beam types 1, 2, 3, 4, and 5 . All other element types continue to use a lumped mass matrix. *CONTROL_IMPLICIT_DYNAMICS_{OPTION} Available options include: <BLANK> DYN SPR Purpose: Activate implicit dynamic analysis and define time integration constants . The DYN option allows setting controls specifically for the dynamic relaxation phase. The SPR option allows setting control specifically for the springback phase. Card 1 1 2 3 4 5 6 7 8 Variable IMASS GAMMA BETA TDYBIR TDYDTH TDYBUR IRATE ALPHA Type Default I 0 F F F F F .50 .25 0.0 1028 1028 I 0 F 0 VARIABLE DESCRIPTION IMASS Implicit analysis type LT.0: curve ID = (-SCALE) used to control amount of implicit TDYBIR, dynamic effects applied to the analysis. TDYDTH and TDYBUR are ignored with this option. EQ.0: static analysis EQ.1: dynamic analysis using Newmark time integration. EQ.2: dynamic analysis by modal superposition following the solution of the eigenvalue problem EQ.3: dynamic analysis by modal superposition using the eigenvalue solution in the d3eigv files that are in the runtime directory. GAMMA Newmark time integration constant . BETA Newmark time integration constant . 100% 0% TDYBIR TDYDTH TDYBUR Time Figure 12-68. Birth, death, and burial time for implicit dynamics. The terms involving 𝑴 and 𝑫 are scaled by a factor between ranging between 1 and 0 to include or exclude dynamical effects, respectively. VARIABLE DESCRIPTION TDYBIR Birth time for application of dynamic terms. See Figure 12-68. TDYDTH Death time for application of dynamic terms. TDYBUR Burial time for application of dynamic terms. IRATE Rate effects switch: EQ.0: rate effects are on in constitutive models EQ.1: rate effects are off in constitutive models EQ.2: rate effects are off in constitutive models for both explicit and implicit. ALPHA Composite time integration constant . GT.0: Bathe composite scheme is activated LT.0: HHT scheme is activated Remarks: For the dynamic problem, the linearized equilibrium equations may be written in the form 𝑴𝒖̈𝑛+1 + 𝑫𝒖̇𝑛+1 + 𝑲𝑡(𝒙𝑛)Δ𝒖 = 𝑷(𝒙𝑛)𝑛+1 − 𝑭(𝒙𝑛) where 𝑴 = lumped mass matrix 𝑫 = damping matrix 𝒖𝑛+1 = 𝒙𝑛+1 − 𝒙0 = nodal displacement vector 𝒖̇𝑛+1 = nodal point velocities at time 𝑛 + 1 𝒖̈𝑛+1 = nodal point acceleration at time 𝑛 + 1 Between the birth and death times 100% of the dynamic terms, that is the terms involving M and D, are applied. Between the death and burial time the dynamic terms are decreased linearly with respect to time until 0% of the dynamic terms are applied after the burial time. This feature is useful for problems that are initially singular because the parts are not in contact initially such as in metal stamping. For these problems dynamics is required for stable convergence. When contact is established the problem becomes well conditioned and the dynamic terms are no longer required for stable convergence. It is recommend that for such problems the user set the death time to be after contact is established and the burial time for 2 or 3 time steps after the death time. For problems with more extensive loading and unloading patterns the user can control the amount of dynamic effects added to the model by using a load curve, see IMASS.LT.0. This curve should have ordinate values between 0.0 and 1.0. The user should use caution in ramping the load curve and the associated dynamic effects from 1.0 to 0.0. Such a ramping down should take place over 2 or 3 implicit time steps. The time integration is by default the unconditionally stable, one-step, Newmark-β time integration scheme 𝒖̈𝑛+1 = Δ𝒖 𝛽Δ𝑡2 − 𝒖̇𝑛 𝛽Δ𝑡 − ( − 𝛽) 𝒖̈𝑛 𝒖̇𝑛+1 = 𝒖̇𝑛 + Δ𝑡(1 − 𝛾)𝒖̈𝑛 + 𝛾Δ𝑡𝒖̈𝑛+1 𝒙𝑛+1 = 𝒙𝑛 + Δ𝒖 Here, Δ𝑡 is the time step size, and 𝛽 and 𝛾 are the free parameters of integration. For 𝛾 = 1 4⁄ the method reduces to the trapezoidal rule and is energy 2⁄ and 𝛽 = 1 conserving. If γ > 𝛽 > + 𝛾) , ( Then numerical damping is induced into the solution leading to a loss of energy and momentum. The Newmark method, and the trapezoidal rule in particular, is known to lack the robustness required for simulating long term dynamic implicit problems. Even though numerical damping may improve the situation from this aspect, it is difficult to know how to set 𝛾 and 𝛽 without deviating from desired physical properties of the system. In the literature, a vast number of composite time integration algorithms have been proposed to handle this, and a family of such methods is implemented and governed by the value of 𝛼 (ALPHA, parameter 8 on card 1). For 𝛼 > 0, every other implicit time step is a three point backward Euler step given as 𝒖̈𝑛+1 = (1 + 𝛼) ∆𝑡 (𝒖̇𝑛+1 − 𝒖̇𝑛) − ∆𝑡− (𝒖̇𝑛 − 𝒖̇𝑛−1) Δ𝒖 − Δ𝒖− 𝒖̇𝑛+1 = (1 + 𝛼) ∆𝑡 ∆𝑡− where ∆𝑡− = 𝑡𝑛 − 𝑡𝑛−1 and Δ𝒖− = 𝒖𝑛 − 𝒖𝑛−1 are constants. Because of this three step procedure, the method is particularly suitable for nodes/bodies undergoing curved motion as it better accounts for curvature than the default Newmark step. For 𝛼 = 1/2, and default values of 𝛾 and 𝛽, the method defaults to the Bathe time integration scheme, Bathe [2007], and is reported to preserve energy and momentum to a reasonable degree. The improvement in stability over the Newmark method is primarily attributed to numerical dissipation, but fortunately this dissipation appears to mainly be due to damping of high frequency content and the underlying physics is therefore not affected as such, see Bathe and Nooh [2012]. For a negative value of ALPHA, the HHT, Hilber-Hughes-Taylor [1977], scheme is activated. This scheme is similar to that of the Newmark method, but the equilibrium is sought at time step 𝑛 + 1 + 𝛼 instead of at 𝑛 + 1. As a complement to the Newmark scheme above, we introduce 𝒖̇𝛼 = −𝛼𝒖̇𝑛 + (1 + 𝛼)𝒖̇𝑛+1 𝒙𝛼 = −𝛼𝒙𝑛 + (1 + 𝛼)𝒙𝑛+1 and solve a modified system of equilibrium equations 𝑴𝒖̈𝑛+1 + 𝑫𝒖̇𝛼 + 𝑭(𝒙𝛼) = 𝑷(𝒙𝛼). 3 ≤ 𝛼 ≤ 0 and 𝛾 = 1−2𝛼 This method is stable for − 1 , which becomes the default values of 𝛾 and 𝛽 if not explicitly set. Parameter 𝛼 controls the amount of dissipation in the problem, for 𝛼 = 0 an undamped Newmark scheme is obtained, whereas 𝛼 = − 1 3 introduces significant damping. From the literature, a value of 𝛼 = −0.05 appears to be a good choice. 2 and 𝛽 = (1−𝛼)2 When modal superposition is invoked, NEIGV on *CONTROL_IMPLICIT_EIGENVAL- UE indicates the number of modes to be used. With modal superposition, stresses are computed only for linear shell formulation 18. *CONTROL_IMPLICIT_EIGENVALUE Purpose: Activate implicit eigenvalue analysis and define associated input parameters . Card 1 1 2 3 4 5 6 7 8 Variable NEIG CENTER LFLAG LFTEND RFLAG RHTEND EIGMTH SHFSCL Type Default I 0 This card is optional. F I F I F I F 0.0 0 -infinity 0 +infinity 2 0.0 Card 2 1 2 3 4 5 6 7 8 Variable ISOLID IBEAM ISHELL ITSHELL MSTRES EVDUMP MSTRSCL Type Default I 0 I 0 I 0 I 0 I 0 I 0 F 0.001 VARIABLE NEIG DESCRIPTION Number of eigenvalues to extract. This must be specified. The other parameters below are optional. LT.0: curve ID = (-NEIG) used for intermittent eigenvalue analysis CENTER This option Center eigenvalues located about this value. frequency. finds the nearest NEIG LFLAG Left end point finite flag. EQ.0: left end point is -infinity EQ.1: left end point is LFTEND. LFTEND Left end point of interval. Only used when LFLAG = 1. VARIABLE DESCRIPTION RFLAG Right end point finite flag: EQ.0: right end point is +infinity EQ.1: right end point is RHTEND. RHTEND Right end point of interval. Only used when RFLAG = 1. EIGMTH Eigenvalue extraction method: EQ.2: Block Shift and Invert Lanczos (default). EQ.3: Lanczos with [M] = [I] (for debug only). EQ.5: Same as 3 but include Dynamic Terms SHFSCL Shift scale. Generally not used, but see explanation below. ISOLID IBEAM ISHELL ITSHELL If nonzero, reset all solid element formulations to ISOLID for the implicit computations. Can be used for all implicit computations not just eigenvalue computations. If nonzero, reset all beam element formulations to IBEAM for the implicit computations. Can be used for all implicit computations not just eigenvalue computations. If nonzero, reset all shell element formulations to ISHELL for the implicit computations. Can be used for all implicit computations not just eigenvalue computations. If nonzero, reset all thick shell element formulations to ITSHELL for the implicit computations. Can be used for all implicit computations not just eigenvalue computations. MSTRES Flag for computing the stresses for the eigenmodes: EQ.0: Do not compute the stresses. EQ.1: Compute the stresses. EVDUMP *CONTROL_IMPLICIT_EIGENVALUE DESCRIPTION Flag for writing eigenvalues and eigenvectors to file “Eigen_ Vectors” (SMP only): EQ.0: Do not write eigenvalues and eigenvectors. GT.0: Write eigenvalues and eigenvectors using an ASCII format. LT.0: Write eigenvalues and eigenvectors using a binary format. MSTRSCL Scaling for computing the velocity based on the mode shape for the stress computation. Remarks: To perform an eigenvalue analysis, activate the implicit method by selecting IM- FLAG = 1 on *CONTROL_IMPLICIT_GENERAL, and indicate a nonzero value for NEIG above. By default, the lowest NEIG eigenvalues will be found. If a nonzero center frequency is specified, the NEIG eigenvalues nearest to CENTER will be found. When NEIG > 0, eigenvalues will be computed at time = 0 and LS-DYNA will terminate. When NEIG < 0, an intermittent eigenvalue analysis will be performed. This is a transient simulation during which loads are applied, with eigenvalues computed periodically during the simulation. Changes in geometry, stress, material, and contact conditions will affect the eigenvalues. The transient simulation can be either implicit or explicit according to IMFLAG = 1 or IMFLAG = 6, respectively, on *CONTROL_IM- PLICIT_GENERAL. The curve ID = -NEIG indicates when to extract eigenvalues, and how many to extract. Define one curve point at each desired extraction time, with a function value equal to the number of eigenvalues desired at that time. A d3plot database will be produced for the transient solution results. Consecutively numbered d3eigv and eigout databases will be produced for each intermittent extraction. The extraction time is indicated in each database’s analysis title. The Block Shift and Invert Lanczos code is from BCSLIB-EXT, Boeing's Extreme Mathematical Library. When using Block Shift and Invert Lanczos, the user can specify a semifinite or finite interval region in which to compute eigenvalues. Setting LFLAG = 1 changes the left end point from -infinity to the value specified by LFTEND. Setting RFLAG = 1 changes the right end point from +infinity to the values given by RHTEND. If the interval includes CENTER (default value of 0.0) then the problem is to compute the NEIG eigenvalues nearest to CENTER. If the interval does not include CENTER, the problem is to compute the smallest in magnitude NEIG eigenvalues. If all of the eigenvalues are desired in an interval where both end points are finite just input a large number for NEIG. The software will automatically compute the number of eigenvalues in the interval and lower NEIG to that value. The most general problem specification is to compute NEIG eigenvalues nearest CENTER in the interval [LFTEND,RHTEND]. Computing the lowest NEIG eigenvalues is equivalent to computing the NEIG eigenvalues nearest 0.0. For some problems it is useful to override the internal heuristic for picking a starting point for Lanczos shift strategy, that is the initial shift. In these rare cases, the user may specify the initial shift via the parameter SHFSCL. SHFSCL should be in the range of first few nonzero frequencies. Parameters CENTER, LFTEND, RHTEND, and SHFSCL are in units of Hertz for eigenvalue problems. These four parameters along with LFLAG and RFLAG are applicable for buckling problems.. For buckling problems CENTER, LFTEND, RHTEND, and SHFSCL are in units of the eigenvalue spectrum. Eigenvectors are written to an auxiliary binary plot database named “d3eigv”, which is automatically created. These can be viewed using a postprocessor in the same way as a standard "d3plot" database. The time value associated with each eigenvector plot is the corresponding frequency in units of cycles per unit time. A summary table of eigenvalue results is printed to the "eigout" file. In addition to the eigenvalue results, modal participation factors and modal effective mass tables are written to the “eigout” file. The user can export individual eigenvectors using LSPrePost. The user can request stresses to be computed and written to d3eigv via MSTRES. A velocity is computed by dividing the displacements from the eigenmode by MSTRSCL. The element routine then computes the stresses based on this velocity, but then those stresses are inversely scaled by MSTRSCL before being written to d3eigv. Thus MSTRSCL has no effect on results of linear element formulations. The strains associated with the stresses output using the MSTRES option can be obtained by setting the STRFLG on *DATABASE_EXTENT_BINARY. Eigenvalues and eigenvectors can be written to file “Eigen_Vectors” by using a nonzero value for EVDUMP. If EVDUMP > 0 an ASCII file is used. If EVDUMP < 0 a simple binary format is used. The binary format is to reduce file space. The eigenvectors written to this file will be orthonormal with respect to the mass matrix. Eigenvector dumping is an SMP only feature. The print control parameter, LPRINT, and ordering method parameter, ORDER, from the *CONTROL_IMPLICIT_SOLVER keyword card also apply to the Block Shift and Invert Eigensolver. *CONTROL_IMPLICIT_FORMING_{OPTION} Available options include: <BLANK> DYN SPR Purpose: This keyword is used to perform implicit static analysis, especially for metal forming processes, such as gravity loading, binder closing, flanging, and stamping subassembly simulation. A systematic study had been conducted to identify the key factors affecting implicit convergence, and the preferred values are automatically set with this keyword. In addition to forming application, this keyword can also be used in other applications, such as dummy loading and roof crush, etc. The DYN option allows setting controls specifically for the dynamic relaxation phase. The SPR option allows setting controls specifically for the springback phase. Card 1 1 2 3 4 5 6 7 8 Variable IOPTION NSMIN NSMAX BIRTH DEATH PENCHK Type Default I 1 I none I 2 F F F 0.0 1.e+20 0.0 VARIABLE DESCRIPTION IOPTION Solution type: EQ.1: Gravity loading simulation, see remarks below. EQ.2: Binder closing and flanging simulation, see remarks below. NSMIN Minimum number of implicit steps for IOPTION = 2. NSMAX Maximum number of implicit steps for IOPTION = 2. BIRTH Birth time to activate this feature. DEATH Death time. DESCRIPTION Relative allowed penetration with respect to the part thickness in contact for IOPTION = 2. time Initial in *CONTROL_IMPLICIT_GENERAL, which is no longer needed if DT0 is specified here. defined size, step as VARIABLE PENCHK DT0 General remarks: This keyword provides a simplified interface for implicit static analysis. If no other implicit cards are used, the stiffness matrix is reformed every iteration. Convergence tolerances (DCTOL, ECTOL, etc.) are automatically set and recommended no to be changed. In almost all cases, only two additional implicit control cards (*CONTROL_- IMPLICIT_GENERAL, and_AUTO) may be needed to control the stepping size, where variables DT0, DTMIN and DTMAX can be used for control. If multiple steps are required for IOPTION = 1, *CONTROL_IMPLICIT_GENERAL must be placed after *CONTROL_IMPLICIT_FORMING with DT0 specified as a certain fraction of the ENDTIM . Otherwise, even with DT0 specified as a fraction of the ENDTIM, only one step (with step size of ENDTIM) will be performed. As always, the variable IGAP should be set to “2” in *CONTACT_FORMING… cards for a more realistic contact simulation in forming. The contact type *CONTACT_- FORMING_SURFACE_TO_SURFACE is recommended to be used with implicit analysis. Smaller penalty stiffness scale factor SLSFAC produces a certain amount of contact penetration but yields faster simulation time, and therefore is recommended for gravity and closing (in case of no physical beads) simulation. Subsequent forming process is likely to follow and contact conditions will be reestablished there, where a tighter, default SLSFAC (0.1) should be used. It is recommended that the fully integrated element type 16 is to be used for all implicit calculation. For solids, type “-2” is recommended. Executable with double precision is to be used for all implicit calculation. Models with over 100,000 deformable elements are more efficient to be simulated with MPP for faster turnaround time. *CONTROL_IMPLICIT_FORMING An example of the implicit gravity is provided below, where a blank is loaded with gravity into a toggle die. A total of five steps are used, controlled by the variable DT0. The results are shown in Figure 12-69. If this binder closing is done with explicit dynamics, efforts need to be made to reduce the inertia effects on the blank since contact with the upper binder only happens along the periphery and a large middle portion of the blank is not driven or supported by anything. With implicit static method, there is no inertia effect at all on the blank during the closing, and no tool speed, time step size, etc. to be concerned about. The implicit gravity application for both air and toggle draw process is available through LS-PrePost 4.0 in Metal Forming Application/eZ Setup (http://ftp.lstc.com/- anonymous/outgoing/lsprepost/4.0/metalforming/). *KEYWORD *PARAMETER ⋮ *CONTROL_TERMINATION 1.0 $---+----1----+----2----+----3----+----4----+----5----+----6----+----7----+----8 *CONTROL_IMPLICIT_FORMING $ IOPTION 1 *CONTROL_IMPLICIT_GENERAL $ IMFLAG DT0 1 0.2 *CONTROL_CONTACT $ SLSFAC RWPNAL ISLCHK SHLTHK PENOPT THKCHG ORIEN 0.03 0.0 2 1 4 0 4 $ USRSTR USRFAC NSBCS INTERM XPENE SSTHK ECDT TIEDPRJ 0 0 10 0 1.0 0 *PART Blank &blkpid &blksec &blkmid *SECTION_SHELL $ SID ELFORM SHRF NIP PROPT QR/IRID ICOMP SETYP &blksec 16 0.833 7 1.0 $ T1 T2 T3 T4 NLOC &bthick,&bthick,&bthick,&bthick *CONTACT_FORMING_SURFACE_TO_SURFACE $ SSID MSID SSTYP MSTYP SBOXID MBOXID SPR MPR &blksid &lpunsid 2 2 1 1 $ FS FD DC VC VDC PENCHK BT DT 0.12 0.0 0.0 0.0 20.0 0 0.0 1E+20 $ SFS SFM SST MST SFST SFMT FSF VSF 1.0 1.0 0.0 &mstp $ SOFT SOFSCL LCIDAB MAXPAR PENTOL DEPTH BSORT FRCFRQ 0 $ PENMAX THKOPT SHLTHK SNLOG ISYM I2D3D SLDTHK SLDSTF 1 $ IGAP IGNORE DPRFAC DTSTIF FLANGL 2 ⋮ *LOAD_BODY_Z 90994 *DEFINE_CURVE_TITLE Body Force on blank 90994 0.0,9810.0 10.0,9810.0 *LOAD_BODY_PARTS &blksid *END Binder closing example: An example of binder closing and its progression is shown in Figures 12-70, 12-71, 12-72, and 12-73, using the NUMISHEET’05 deck lid inner, where a blank is being closed in a toggle die (modified). An adaptive level of three was used in the closing process. Gravity is and should be always applied at the same time, regardless if a prior gravity loading simulation is performed or not, as listed at the end of the input deck. The presence of the gravity helps the blank establish an initial contact with the tool, thus improving the convergence rate. The upper binder is moved down by a closing distance (defined by a parameter &bindmv) using a displacement boundary condition (VAD = 2), with a simple linearly increased triangle-shaped load curve. The variable DT0 is set at 0.01, determined by the expected total deformation. The solver will automatically adjust based on the initial contact condition. The maximum step size is controlled by the variable DTMAX, and this value needs to be sufficiently small (<0.02) to avoid missing contact, but yet not too small causing a long running time. In some cases, this variable can be set larger, but the current value works for most cases. *KEYWORD *PARAMETER ⋮ *CONTROL_TERMINATION 1.0 *CONTROL_IMPLICIT_FORMING $ IOPTION NSMIN NSMAX 2 2 100 *CONTROL_IMPLICIT_GENERAL $ IMFLAG DT0 1 0.01 *CONTROL_IMPLICIT_AUTO $ IAUTO ITEOPT ITEWIN DTMIN DTMAX 0 0 0 0.01 0.03 *CONTROL_ADAPTIVE ⋮ *CONTROL_CONTACT $ SLSFAC RWPNAL ISLCHK SHLTHK PENOPT THKCHG ORIEN 0.03 0.0 2 1 4 0 4 $ USRSTR USRFAC NSBCS INTERM XPENE SSTHK ECDT TIEDPRJ 0 0 10 0 1.0 0 $---+----1----+----2----+----3----+----4----+----5----+----6----+----7----+----8 ⋮ *PART Blank $ PID SECID MID EOSID HGID GRAV ADPOPT TMID &blkpid &blksec &blkmid &adpyes *SECTION_SHELL $ SID ELFORM SHRF NIP PROPT QR/IRID ICOMP SETYP &blksec 16 0.833 7 1.0 $ T1 T2 T3 T4 NLOC &bthick,&bthick,&bthick,&bthick ⋮ *CONTACT_FORMING_SURFACE_TO_SURFACE $ SSID MSID SSTYP MSTYP SBOXID MBOXID SPR MPR &blksid &lpunsid 2 2 1 1 $ FS FD DC VC VDC PENCHK BT DT 0.12 0.0 0.0 0.0 20.0 0 0.0 1E+20 $ SFS SFM SST MST SFST SFMT FSF VSF 1.0 1.0 0.0 &mstp $ SOFT SOFSCL LCIDAB MAXPAR PENTOL DEPTH BSORT FRCFRQ 0 $ PENMAX THKOPT SHLTHK SNLOG ISYM I2D3D SLDTHK SLDSTF 1 $ IGAP IGNORE DPRFAC DTSTIF FLANGL 2 *CONTACT_... $---+----1----+----2----+----3----+----4----+----5----+----6----+----7----+----8 *BOUNDARY_PRESCRIBED_MOTION_RIGID $ typeID DOF VAD LCID SF VID DEATH BIRTH &bindpid 3 2 3 -1.0 0 *DEFINE_CURVE 3 0.0,0.0 1.0,&bindmv $---+----1----+----2----+----3----+----4----+----5----+----6----+----7----+----8 $ Activate gravity on blank: *LOAD_BODY_Z 90994 *DEFINE_CURVE_TITLE Body Force on blank 90994 0.0,9810.0 10.0,9810.0 *LOAD_BODY_PARTS &blksid *END Binder closing with real beads example: Binder closing with real beads can also be done with implicit static, and with adaptive mesh. An example is shown in Figure 12-74, where a hood outer is being closed implicitly. It is noted a small buckle can be seen near the draw bead region along the fender line. These kind of small forming effects can be more accurately detected with implicit static method. The implicit static closing can now be set up in LS-PrePost v4.0 Metal Forming Application/eZ Setup (http://ftp.lstc.com/anonymous/outgoing/lsprepost/4.0/metal- forming/). Flanging example: An example of flanging simulation using this feature is shown in Figures 12-75, 12-76 and 12-77, with NUMISHEET’02 fender outer, where flanging is conducted along the hood line. A partial input is provided below, where DTMAX is controlled by a load curve for contact and speed. The use of DTMAX with a load curve is an exception to the rule, where most of the time this is not needed. Smaller step sizes are better in some cases than larger step sizes, which may take longer to converge resulting from cutbacks in step sizes. Gravity, pad closing and flanging were set to 10%, 10% and 80% of the total step size, respectively. Pad travels a distance of ‘&padtrav’ starting at 0.1, when it is to be automatically moved to close the gap with the blank due to gravity loading (*CONTACT_AUTO_MOVE), and finishing at 0.2 and held in that position until the end. Flanging steel travels a distance of ‘&flgtrav’ starting at 0.2 and completing at 1.0. A detailed section view of the simulation follows in Figure 12-78. *KEYWORD *PARAMETER ... *CONTROL_TERMINATION 1.0 *CONTROL_IMPLICIT_FORMING $ IOPTION NSMIN NSMAX 2 2 200 *CONTROL_IMPLICIT_GENERAL 1 0.100 *CONTROL_IMPLICIT_AUTO $ IAUTO ITEOPT ITEWIN DTMIN DTMAX 0 0 0 0.005 -9980 *DEFINE_CURVE 9980 0.0,0.1 0.1,0.1 0.2,0.1 0.7,0.005 1.0,0.005 *CONTROL_ADAPTIVE... *CONTROL_CONTACT... *PART... *SECTION_SHELL... *CONTACT_... *CONTACT_FORMING_SURFACE_TO_SURFACE_ID_MPP 2 0,200,,3,2,1.005 $ SSID MSID SSTYP MSTYP SBOXID MBOXID SPR MPR &blksid &padsid 2 2 $ FS FD DC VC VDC PENCHK BT DT 0.12 0.0 0.0 0.0 20.0 0 0.0 1E+20 $ SFS SFM SST MST SFST SFMT FSF VSF 1.0 1.0 0.0 &mstp $ SOFT SOFSCL LCIDAB MAXPAR PENTOL DEPTH BSORT FRCFRQ 0 $ PENMAX THKOPT SHLTHK SNLOG ISYM I2D3D SLDTHK SLDSTF 1 $ IGAP IGNORE DPRFAC DTSTIF FLANGL 2 *BOUNDARY_PRESCRIBED_MOTION_RIGID $ typeID DOF VAD LCID SF VID DEATH BIRTH &padpid 3 2 3 -1.0 0 &flgpid 3 2 4 -1.0 0 *DEFINE_CURVE 3 0.0,0.0 0.1,0.0 0.2,&padtrav 1.0,&padtrav *DEFINE_CURVE 4 0.0,0.0 0.2,0.0 1.0,&flgtrav $ Activate gravity on blank: *LOAD_BODY_PARTS &blksid *LOAD_BODY_Z 90994 *DEFINE_CURVE_TITLE Body Force on blank 90994 0.0,9810.0 10.0,9810.0 *CONTACT_AUTO_MOVE $ ID ContID VID LCID ATIME -1 2 89 3 0.1 *END Flanging simulation using IOPTION of 1: IOPTOIN 1 can also be used for closing and flanging simulation, or other applications that go through large plastic strains or deformation. This is used when an equal step size throughout the simulation is desired, and is done by specifying the equal step size in the variable DT0 in *CONTROL_IMPLICIT_GENERAL, as shown in the following keywords (other cards similar and not included), where DT0 of 0.014 is chosen. Such an application is shown in Figures 12-79 and 12-80. *CONTROL_TERMINATION 1.0 *CONTROL_IMPLICIT_FORMING $ IOPTION 1 *CONTROL_IMPLICIT_GENERAL $ IMFLAG DT0 1 0.014 Switching between implicit dynamic and implicit static for gravity loading: For sheet blank gravity loading, it is now possible to start the simulation using implicit dynamic method, switching to implicit static method at a user defined time until completion. This feature is activated by setting the variable TDYDTH in *CONTROL_- IMPLICIT_DYNAMICS and was recently (Rev. 81400) linked together with *CON- TROL_IMPLICIT_FORMING. In a partial keyword example below, death time for the implicit dynamic is set at 0.55 second. The test model shown in Figure 12-81 (left) results in a gravity loaded blank shape in Figure 12-81 (right). Without the switching, the blank will look like as shown in Figure 12-82. The gravity loaded blank shape is more reasonable with the switching. A check on the energy history reveals that the kinetic energy dissipated completely at 0.60 second, Figure 12-83. *CONTROL_TERMINATION 1.0 *CONTROL_IMPLICIT_FORMING $ IOPTION NSMIN NSMAX BIRTH DEATH PENCHK 1 *CONTROL_IMPLICIT_DYNAMICS $ IMASS GAMMA BETA TDYBIR TDYDTH TDYBUR IRATE 1 0.600 0.380 0.55 Revision information: This implicit capability is available in R5.0 and later releases. This keyword is implemented in LS-PrePost4.0 eZSetup for metal forming application. 1)Revision 64802: Multi-step gravity loading simulation. 2)Revision 81400: Switching feature between implicit dynamic and implicit static. 3)Revision 104837: variable DT0. Time= 1 Contours of Z-displacement Original flat sheet blank after auto-position Z-displacement (mm) Gravity-loaded blank Binder opening Lower binder 7.01 -31.92 -70.86 -109.80 -148.70 -187.70 -226.60 -265.50 -304.50 -343.40 -382.30 Figure 12-69. Gravity loading on a box side outer toggle die (courtesy of Autodie, LLC). Figure 12-70. Initial auto-positioning (NUMISHEET2005 decklid inner). Figure 12-71. At 50% upper travel. Figure 12-72. At 80% upper travel. Figure 12-73. Upper travels to home. Draw beads Blank shape upon binder closing Upper cavity Buckles predicted Blank Lower binder (with contact offset of 1.1x blank thickness) Figure 12-74. Binder closing with beads on a hood outer. Section A-A Figure 12-75. Mean stress at pad closing. Figure 12-76. Mean stress at 40% Travel. B Home (view 1) Home (view 2) Figure 12-77. Mean stress at flanging home (compression/surface lows in red). Upper pad Flanging post Trimmed panel Flanging steel Figure 12-78. Flanging progression along section B (flanging post stationary). Thinning (%) 20.0 18.0 16.0 14.0 12.0 10.0 8.0 6.0 4.0 2.0 0.0 Flanged area in detail next figure Figure 12-79. Flanging simulation of a rear floor pan using IOPTION 1 (Courtesy of Chrysler, LLC). Thinning (%) 20.0 Pressure (MPa) 294.1 18.0 16.0 14.0 12.0 10.0 8.0 6.0 4.0 2.0 -0.0 Thinning contour 235.9 177.7 119.5 61.25 3.03 -55.2 -113.4 -171.6 -229.8 -288.1 Mean stress contour - compression in red Figure 12-80. Localized view of the last figure. Initial totally flat sheet blank Binder Time=0 Time=1.0 Figure 12-81. Test model (left) and gravity loaded blank (right) with switching from implicit dynamic to implicit static. Figure 12-82. Gravity loaded blank without the “switching”. Time=1.0 25 20 15 10 ) ( 0.0 t=0.55 t=0.60 Implicit dynamic Implicit static Kinetic energy Internal energy Total energy Kinetic energy dissipates after a small transition step 0.2 0.4 0.6 0.8 1.0 Implicit "time" (sec.) Figure 12-83. Switching between implicit dynamic and implicit static. *CONTROL_IMPLICIT_GENERAL_{OPTION} Availlable option s include: <BLANK> DYN SPR Purpose: Activate implicit analysis and define associated control parameters. This keyword is required for all implicit analyses. The DYN option allows setting controls specifically for the dynamic relaxation phase. The SPR option allows setting controls specifically for the springback phase. Card 1 1 2 3 4 5 6 7 8 Variable IMFLAG DT0 IMFORM NSBS IGS CNSTN FORM ZERO_V Type Default I 0 F none I 2 I 1 I 2 I 0 I 0 I 0 VARIABLE DESCRIPTION IMFLAG Implicit/Explicit analysis type flag EQ.0: explicit analysis EQ.1: implicit analysis EQ.2: explicit followed by implicit, (seamless springback). *IN- to is required TERFACE_SPRINGBACK_SEAMLESS activate seamless springback. EQ.4: implicit with automatic implicit-explicit switching EQ.5: implicit with automatic switching and mandatory implicit finish EQ.6: explicit with intermittent eigenvalue extraction LT.0: curve ID = -IMGFLAG specifies IMFLAG as a function of time. DT0 Initial time step size for implicit analysis Implicit 1 Explicit 0 Figure 12-84. Solution method, implicit or explicit, controlled by a load curve. Time VARIABLE IMFORM DESCRIPTION Element formulation flag for seamless springback; see *INTER- FACE_SPRINGBACK_SEAMLESS. EQ.1: switch to springback fully integrated shell formulation for EQ.2: retain original element formulation (default) NSBS Number of implicit steps in seamless springback; see *INTER- FACE_SPRINGBACK_SEAMLESS. IGS Geometric (initial stress) stiffness flag EQ.1: include EQ.2: ignore CNSTN Indicator for consistent tangent stiffness (solid materials 3 & 115 only): EQ.0: do not use (default) EQ.1: use. FORM integrated element Fully IMFORM = 1 only) formulation (IMFLAG = 2 and EQ.0: type 16 EQ.1: type 6. VARIABLE DESCRIPTION ZERO_V Zero out the velocity before switching from explicit to implicit. EQ.0: The velocities are not zeroed out. EQ.1: The velocities are set to zero. Remarks: VARIABLE IMFLAG REMARK The default value 0 indicates a standard explicit analysis will be performed. Using value 1 causes an entirely implicit analysis to be performed. Value 2 is automatically activated when the keyword *INTERFACE_SPRINGBACK_SEAMLESS is present, causing the analysis type to switch from explicit to implicit when the termination time is reached. Other nonzero values for IM- FLAG can also be used with *INTERFACE_SPRINGBACK_- SEAMLESS. After this switch, the termination time is extended by NSBS*DT0, or reset to twice its original value if DT0 = 0.0. The implicit simulation then proceeds until the new termination time is reached. Contact interfaces are automatically disabled during the implicit phase of seamless springback analysis. Furthermore, implicit stabilization (*CONTROL_IMPLICIT_STABILIZATION) and automatic step size adjustment (*CONTROL_IMPLICIT_AU- TO) on by default for seamless springback. When the automatic implicit-explicit switching option is activated (IMFLAG = 4 or 5), the solution method will begin as implicit. If convergence of the equilibrium iterations fails, the solution will automatically switch to explicit for a time interval of DTEXP . After this time interval, the solution method will switch back to implicit and attempt to proceed. The implicit simulation may be either static or dynamic. When this feature is used in a static implicit job, simulation time is no longer arbitrary, and must be chosen along with DTEXP in a realistic way to allow efficient execution of any explicit phases. Mass scaling may also be activated , and will apply only during the explicit phases of the calculation. In cases where much switching occurs, users must exercise caution to ensure that negligible dynamic effects are introduced by the explicit phases. When IMFLAG = 5, the final step of the simulation must be implicit. The termination time will be extended automatically as necessary, until a successfully converged implicit step can be VARIABLE REMARK obtained. This is useful for example in difficult metal forming springback simulations. When IMFLAG = 6, an explicit simulation will be performed. Eigenvalues will be extracted intermittently according to a curve indicated by NEIG=(-curve ID) on *CONTROL_IMPLICIT_- EIGENVALUE. Beware that dynamic stress oscillations which may occur in the explicit simulation will influence the geometric (initial stress) stiffness terms used in the eigen solution, potentially producing misleading results and/or spurious modes. As an alternative, eigenvalues can also be extracted intermittently during an implicit analysis, using IMFLAG = 1 and NEIG=(-curve ID). When IMFLAG < 0, a curve ID is indicated which gives the solution method as a function of time. Define a curve value of zero during explicit phases, and a value of one during implicit phases. Use steeply sloping sections between phases. An arbitrary number of formulation switches may be activated with this method. See Figure 12-84. This parameter selects the initial time step size for the implicit phase of a simulation. The step size may change during a multiple step simulation if the automatic time step size control feature is active Adaptive mesh must be activated when using element formulation switching. For best springback accuracy, use of shell type 16 is recommended during the entire stamping and springback analysis, in spite of the increased cost of using this element during the explicit stamping phase. The NSBS option allows a seamless springback analysis, invoked with *INTERFACE_SPRINGBACK_SEAMLESS, to use multiple unloading steps. Implicit seamless springback beings at time, 𝑡 = ENDTIM and finishes at 𝑡 = ENDTIM + NSBS × DT0 were ENDTIM is specified in *CONTROL_TERMINATION and DT0 is specified in *CONTROL_IMPLICIT_GENERAL. The geometric stiffness adds the effect of initial stress to the global stiffness matrix. This effect is seen in a piano string whose natural frequency changes with tension. Geometric stiffness does not always improve nonlinear convergence, especially when DT0 INFORM NSBS IGS VARIABLE REMARK compressive stresses are present, so its inclusion is optional. Furthermore, the geometric stiffness may lead to convergence incompressible, incompressible, or nearly problems with materials. *CONTROL_IMPLICIT_INERTIA_RELIEF Purpose: Allows analysis of linear static problems that have rigid body modes. Card 1 1 2 3 4 5 6 7 8 Variable IRFLAG THRESH IRCNT Type Default I 0 F 0.001 I 0 Additional Mode List Cards. This card should be included only when the user wants to specify the modes to use. Include as many cards as needed to provide all values. This input ends at the next keyword (“*”) card. The mode numbers do not have to be consecutive. Card 2 1 2 3 4 5 6 7 8 Variable MODE1 MODE2 MODE3 MODE4 MODE5 MODE6 MODE7 MODE8 Type I I I I I I I I VARIABLE DESCRIPTION IRFLAG Inertia relief flag EQ.0: do not perform inertia relief EQ.1: do perform inertia relief THRESH Threshold for what is a rigid body mode. The default is set to 0.001 Hertz where it is assumed that the units are in seconds. IRCNT MODEi The user can specify to use the lowest IRCNT modes instead of using THRESH to determine the number of modes. Ignore THRESH and IRCNT and use a specific list of modes, skipping those that should not be used. *CONTROL Purpose: Specify penalty or constraint treatment of joints for implicit analysis. Card 1 1 2 3 4 5 6 7 8 Variable ISPHER IREVOL ICYLIN Type Default I 1 I 1 I 1 VARIABLE DESCRIPTION ISPHER Treatment of spherical joints EQ.1: use constraint method for all spherical joints (default) EQ.2: use penalty method for all spherical joints IREVOL Treatment of revolute joints EQ.1: use constraint method for all revolute joints (default) EQ.2: use penalty method for all revolute joints ICYLIN Treatment of cylindrical joints EQ.1: use constraint method for all cylindrical joints (default) EQ.2: use penalty method for all cylindrical joints Remarks: For most implicit applications one should use the constraint (default) method for the treatment of joints. When explicit-implicit switching is used the joint treatment should be consistent. This keyword allows the user to choose the appropriate treatment for their application. *CONTROL_IMPLICIT_MODAL_DYNAMIC Purpose: Activate implicit modal dynamic analysis. Eigenmodes are used to linearize the model by projecting the model onto the space defined by the eigenmodes. The eigenmodes can be computed or read from a file. All or some of the modes can be used in the linearization. Modal damping can be applied. Card 1 1 2 3 4 5 6 7 8 Variable MDFLAG ZETA Type I F Optional Filename Card. Card 2 1 2 3 4 5 6 7 8 Variable Type FILENAME A80 VARIABLE DESCRIPTION MDFLAG Modal Dynamic flag EQ.0: no modal dynamic analysis EQ.1: perform modal dynamic analysis. ZETA Modal Dynamic damping constant. FILENAME If specified the eigenmodes are read from the specified file. Otherwise the eigenmodes are computed as specified on *CON- TROL_IMPLICIT_EIGENVALUE. Remarks: Modal Dynamic uses the space spanned by the eigenmodes of the generalized eigenvalue problem The matrix of eigenmodes, 𝚽, diagonalizes 𝐊 and 𝐌 𝐊𝛟𝑖 = 𝜆𝑖𝐌𝛟𝑖. 𝚽𝐓𝐊𝚽 = 𝚲 and 𝚽𝐓𝐌𝚽 = 𝐈. Multiplication by 𝜱 changes coordinates from amplitude space to displacement space as where 𝒂 is a vector of modal amplitudes. The equations of motion 𝐌𝐮̈𝑛+1 + 𝐊𝚫𝐮 = 𝐅(𝐱𝒏) 𝐮 = 𝚽𝐚 when multiplied on the left by 𝛟T and substituting 𝐮 = 𝚽𝐚 become the linearized equations of motion in its spectral form as, 𝐈𝐚̈𝑛+1 + 𝚲(𝚫𝐚) = 𝚽T𝐅(𝐱𝑛). The modal damping features adds a velocity dependent damping term, 𝐈𝐚̈𝑛+1 + 2𝐙𝐚̇𝑛 + 𝚲(𝚫𝐚) = 𝚽T𝐅(𝐱𝒏) Where 𝑍𝑖𝑖 = 𝜁𝑖𝜔𝑖, 𝜔𝑖 = √𝜆𝑖, and each 𝜁𝑖 is a user specified damping coefficients. The matrices in the reduced equations are diagonal and constant. So Modal Dynamics can quickly compute the acceleration of the amplitudes and hence the motion of the model. But the motion is restricted to the space spanned by the eigenmodes. Eigenmodes are either computed based on *CONTROL_IMPLICIT_EIGENVALUE or read from file FILENAME. By default all modes are used in the projection. Selected modes can be specified via *CONTROL_IMPLICIT_MODAL_DYNAMIC_MODE to reduce the size of the projection. . Stresses are computed only for linear shell formulation 18 and linear solid formulation 18. Modal damping on all modes can be specified using ZETA. More options for specifying modal damping can be found on *CONTROL_IMPLICIT_MODAL_DYNAMIC_DAMP- ING. Using MDFLAG = 1, ZETA = 0.0, and FILENAME = “ ” is the same as using IMASS = 2 with *CONTROL_IMPLICIT_DYNAMICS. Using MDFLAG = 1, ZETA = 0.0 and FILE- NAME = ’d3eigv’ is the same as IMASS = 3. The new keywords *CONTROL_IMPLIC- IT_MODAL_DYNAMIC_MODE and *CONTROL_IMPLICIT_MODAL_DYNAMIC_- DAMPING provide additional user options for mode selection and modal damping. *CONTROL_IMPLICIT_MODAL_DYNAMIC_DAMPING_{OPTION} Available options include: BLANK SPECIFIC FREQUENCY_RANGE Purpose: Define vibration modes to be used in implicit modal dynamic. Damping Card. Card for option set to <BLANK>. Card 1 1 2 3 4 5 6 7 8 Variable ZETA1 Type F I Specific Damping Cards. Cards for the SPECIFIC option. This input ends at the next keyword (“*”) card. Card 1 1 2 3 4 5 6 7 8 Variable MID1 ZETA1 MID2 ZETA2 MID3 ZETA3 MID4 ZETA4 Type I F I F I F I F Frequency Range Damping Cards. Cards for FREQUENCY_RANGE option. This input ends at the next keyword (“*”) card. Card 1 1 2 3 4 5 6 7 8 Variable FREQ1 ZETA1 FREQ2 ZETA2 FREQ3 ZETA3 FREQ4 ZETA4 Type F F F F F F F F VARIABLE DESCRIPTION ZETAn Modal Dynamic damping coefficient n. MIDn Mode ID n. f1 f2 f3 f4 f5 frequency Figure 12-85. Schematic illustration of frequency range damping. VARIABLE DESCRIPTION FREQn Frequency value n. Remarks: 1. 2. 3. If no option is specified the value of ZETA1 becomes the damping coefficient for all modes involved in implicit modal dynamic analysis. This value over- rides the value on *CONTROL_IMPLICIT_MODAL_DYNAMIC. If option SPECIFIC is specified the integers MIDn indicate which modes involved in *CONTROL_IMPLICIT_MODAL_DYNAMIC will have modal damping applied to them. The associated value ZETAn will be the modal damping coefficient for that mode. If option FREQUENCY_RANGE is specified all modes involve will have modal damping applied. The damping coefficient will be computed by linear interpo- lation of the pairs (FREQi, ZETAi). If the modal frequency is less than FREQ1 then the modal damping coefficient will be ZETA1. If the modal frequency is greater than FREQn then the modal damping coefficient will be ZETAn. The values of FREQi must be specified in ascending order. *CONTROL_IMPLICIT_MODAL_DYNAMIC_MODE_OPTION Available options include: LIST GENERATE Purpose: Define vibration modes to be used in implicit modal dynamic. Mode ID Cards. Card 1 for the LIST keyword option. For each mode include an addition. This input ends at the next keyword (“*”) card. Card 1 1 2 3 4 5 6 7 8 Variable MID1 MID2 MID3 MID4 MID5 MID6 MID7 MID8 Type I I I I I I I I Mode Range Cards. Card 1 for the GENERATE keyword option. For each range of modes include an additional card. This input ends at the next keyword (“*”) card. Card 1 1 2 3 4 5 6 7 8 Variable M1BEG M1END M2BEG M2END M3BEG M3END M4BEG M4END Type I I I I I I I I VARIABLE DESCRIPTION MIDn Mode ID n. MnBEG First mode ID in block n. MnEND Last mode ID in block n. All mode ID’s between and including MnBEG and MnEND are added to the list. Remarks: 1. User may use this keyword with *CONTROL_IMPLICIT_MODAL_DYNAMIC if some of the vibration modes have less contribution to the total structural response and can be removed from the implicit modal dynamic analysis. *CONTROL_IMPLICIT_MODES_{OPTION} Available options include: <BLANK> BINARY Purpose: Request calculation of constraint, attachment, and/or eigenmodes for later use in modal analysis using *PART_MODES or *ELEMENT_DIRECT_MATRIX_INPUT. Card 1 1 2 3 4 5 6 7 8 Variable NSIDC NSIDA NEIG IBASE SE_MASS SE_DAMP SE_STIFF SE_INERT I 0 2 Type Default I 0 Card 2 1 Variable Type I I C C C C 3 4 5 6 7 8 SE_FILENAME C VARIABLE DESCRIPTION NSIDC Node set ID for constraint modes EQ.0: no constraint modes will be generated NSIDA Node set ID for attachment modes EQ.0: no attachment modes will be generated NEIG Number of eigenmodes (normal modes) EQ.0: no eigenmodes will be generated IBASE Offset for numbering of the generalized internal degrees of freedom for the superelement SE_MASS *CONTROL_IMPLICIT_MODES DESCRIPTION Name of the superelement mass matrix. If left blank it is not generated. SE_DAMP Name of the superelement damping matrix. If left blank it is not generated. SE_STIFF Name of the superelement stiffness matrix. If left blank it is not generated. SE_INERT Name of the superelement inertia matrix, required for gravity loading applications of the superelement. If left blank it is not generated. SE_FILENAME If any of SE_MASS, SE_DAMP, SE_STIFF, or SE_INERT are not blank then the second line is required and contains the file name for the superelement. Remarks: To use this feature, an implicit analysis must be requested using IMFLAG = 1 on *CON- TROL_IMPLICIT_GENERAL, and a non-zero termination time must be specified on *CONTROL_TERMINATION. A double precision version of LS-DYNA should be used for best accuracy. Care must be taken to apply a sufficient number of constraints to the model to eliminate static rigid body motion. Computed modes are written to binary output file d3mode, with the order of output being constraint modes, followed by attachment modes, and then eigenmodes. The d3mode file can be read and modes viewed using LS-PrePost. Eigenmodes are also written to binary output file d3eigv. Constraint and attachment modes are generated by applying unit displacements and unit forces, respectively, to each specified degree of freedom. By default, modes are computed for all degrees of freedom for each node in sets NSIDC and NSIDA. The first and second node set attribute parameters can be optionally used to restrict the translational and rotational degrees of freedom for which modes are requested, respectively, according to the following syntax: Node set attribute parameters DA1 and A1: translational degree of freedom codes Node set attribute parameters DA2 and A2: rotational degree of freedom codes code modes computed X degree of freedom only Y degree of freedom only 0 1 3 4 5 6 7 Z degree of freedom only X, Y degrees of freedom only Y, Z degrees of freedom only X, Z degrees of freedom only X, Y, Z degrees of freedom Setting both node set attributes to zero is equivalent to setting both node set attributes to 7 (X, Y, and Z for translational and rotational degrees of freedom). If one node set attribute is nonzero (codes 1 to 7) and the other node set attribute is zero, then the zero attribute means NO degrees of freedom are considered. For example, if DA1 = 2 and DA2 = 0, then only the Y-translational degree of freedom modes are calculated. Eigenmodes are generated for the model with single point constraints applied on the constraint modes. The number of eigenmodes is specified here. If the user wants to compute eigenmodes other than the lowest ones, the controls on *CONTROL_IMPLIC- IT_EIGENVALUE can be used. When the superelement is created an internal numbering must be applied to the attachment and eigen modes. This numbering starts at IBASE+1. The user can create the superelement representation of the reduced model by specifying the SE_MASS, SE_DAMP, SE_STIFF, SE_INERT and SE_FILENAME fields. The inertia matrix is necessary if body forces, e.g., gravity loads, are applied to the superelement. The file, by default is written in the Nastran DMIG file format and can be used as input to *ELEMENT_DIRECT_MATRIX_INPUT. The BINARY keyword option can be used to create a binary representation for the superelement which can be used with *ELE- MENT_DIRECT_MATRIX_INPUT_BINARY to reduce the file size. The combination of constraint modes and eigenmodes form the Hurty-Craig-Bampton linearization for a model. Using only constraint modes is the same as static condensation. Some broad guidelines for appropriate selection of constraint modes, attachment modes, and eigenmodes include: 1. Use constraint modes for the nodal degrees-of-freedom that are to be "con- strained" with SPCs or prescribed motion. 2. Use attachment modes for nodal degrees-of-freedom that are under the influence of point loads. 3. Use eigenmodes in the construction of the superelement to capture the reaction of the part being modeled by the superelement and the associated feedback to the rest of the model. *CONTROL_IMPLICIT_ROTATIONAL_DYNAMICS Purpose: This keyword is used to model rotational dynamics using the implicit time integrator. Applications for this feature include the transient and vibration analysis of rotating parts such as turbine blades, propellers in aircraft, and rotating disks in hard disk drives. The current implementation requires a double-precession SMP version of LS-DYNA. An MPP implementation is under development. Card 1 1 2 3 4 5 6 7 8 Variable SID STYPE OMEGA VID NOMEG IREF OMEGADR Type I Default none I 0 F I none none I 0 I 0 F 0 Additional Rotational Speed Cards. This card should be included only when NOMEG > 0. Include as many cards as needed to provide all NOMEG values. This input ends at the next keyword (“*”) card. Card 2 1 2 3 4 5 6 7 8 Variable OMEG1 OMEG2 OMEG3 OMEG4 OMEG5 OMEG6 OMEG7 OMEG8 Type F F F F F F F F VARIABLE DESCRIPTION SID Set ID of the rotational components. STYPE Set type: EQ.0: Part; EQ.1: Part set. OMEGA Rotating speed. GT.0: rotating speed. LT.0: curve ID = (-OMEGA) gives rotating speed as a function of time. VID *CONTROL_IMPLICIT_ROTATIONAL_DYNAMICS DESCRIPTION Vector ID to define the rotating axis. It can be defined in *DE- FINE_VECTOR and *DEFINE_VECTOR_NODES, and the tail of the vector should be set as the rotating center. NOMEG Number of rotating speeds. This feature is intended to automatically preform parameter studies with respect to the rotation speed. The keyword *CONTROL_IMPLICIT_EIGEN- VALUE must be included if NOMEG > 0. IREF Reference frame: EQ.0: Rotating coordinate system and rotating parts will not rotate in visualization. Solid element and thick shell element will use IREF = 0. EQ.1: Fixed coordinate system. Rotating parts rotates and the initial rotating velocity should be defined in *INITIAL_- VELOCITY_GENERATION as well. EQ.2: Rotating coordinate system, but rotate rotating parts for visualization purpose. OMEGn The nth rotating speed. OMEGADR Rotating speed defined in dynamic relaxation. GT.0: rotating speed defined in dynamic relaxation. LT.0: curve ID = (-OMEGA) gives rotating speed as a function of time. Remarks: The linearized equilibrium equation in the rotating coordinate system is given by Whereas, in a fixed coordinate system, the linearized equilibrium equation is 𝐌𝐮̈ + (𝐃 + 2Ω𝐂)𝒖̇ + (𝑲 − Ω2𝐊𝐺)𝐮 = 𝐅 𝐌𝐮̈ + (𝐃 + Ω𝐂)𝐮̇ + 𝐊𝐮 = 𝐅 with 𝐌 = lumped mass matrix 𝐃 = damping matrix 𝐊 = stiffness matrix 𝐂 = gyroscopic matrix 𝐊𝐺 = centrifugal stiffness matrix 𝐮 = nodal displacement vector 𝐮̇ = nodal point velocities at time 𝐮̈ = nodal point acceleration at time Ω = rotating speed The chief difference between the equations for the rotating and fixed frames is the inclusion of the centrifugal stiffness matrices𝐊𝑔. Additionally, the coefficient on the gyroscopic matrix, 𝐂, as well as its content are modified in the rotating-frame case. Specifically, the rotating system includes an additional Coriolis contribution to 𝐂. In many applications of rotational dynamics, the critical speed – the theoretical angular velocity that excites the natural frequency of a rotating object – is of particular concern. Therefore, the study of mode frequency response with the change of the rotating speed is very important. The Campbell diagram, which is defined to represent a system’s eigen-frequencies as a function of rotating speeds, is introduced for this purpose. In order to do this, the user needs to define a set of rotating speeds on card 2, and LS- DYNA will do modal analysis for each of these speeds. NOMEG should be defined as the number of rotating speeds used in card 2. A keyword file example in this application can be set as follows: *KEYWORD *CONTROL_TERMINATION... *CONTROL_IMPLICIT_EIGENVALUE 5 *CONTROL_IMPLICIT_GENERAL 1 0.05 *CONTROL_IMPLICIT_ROTATIONAL_DYNAMICS $# SID STYPE OMEGA VID NOMEGA IREF 1 0 0.0 1 4 1 $# OMEG1 OMEG2 OMEG3 OMEG4 50.0 100.0 150.0 200.0 *DEFINE_VECTOR $# VID XT YT ZT XH YH ZH CID 1 0.0 0.0 0.0 1.0 0.0 0.0 *DATABASE_... *PART... *SECTION... *MAT... *ELEMENT... *NODE... *END Besides of modal analysis, transient analysis can also be done using this keyword. A keyword file example can be set as follows: *KEYWORD *CONTROL_TERMINATION... *CONTROL_IMPLICIT_GENERAL 1 0.05 *CONTROL_IMPLICIT_ROTATIONAL_DYNAMICS $# SID STYPE OMEGA VID NOMEGA IREF 1 0 0.0 1 0 0 *DEFINE_VECTOR $# VID XT YT ZT XH YH ZH CID 1 0.0 0.0 0.0 1.0 0.0 0.0 *DATABASE_... *PART... *SECTION... *MAT... *ELEMENT... *NODE... *END *CONTROL_IMPLICIT_SOLUTION_{OPTION} Available options include: <BLANK> DYN SPR Purpose: These optional cards apply to implicit calculations. Use these cards to specify whether a linear or nonlinear solution is desired. Parameters are also available to control the implicit nonlinear and arc length solution methods . The DYN option allows setting controls specifically for the dynamic relaxation phase. The SPR option allows setting controls specifically for the springback phase. Card 1 1 2 3 4 5 6 7 8 Variable NSOLVR ILIMIT MAXREF DCTOL ECTOL RCTOL LSTOL ABSTOL Type I I I F F F F F Default 12 11 15 0.001 0.01 1010 0.90 10-10 Remaining cards are optional.† Optional 2a 1 2 3 4 5 6 7 8 Variable DNORM DIVERG ISTIF NLPRINT NLNORM D3ITCTL CPCHK Type Default I 2 I 1 I 1 I 0 F/I 2 I 0 I 0 Strict Tolerances Optional Card. Define this card if and only if DNORM.LT.0 Optional 2b 1 2 3 4 5 6 7 8 Variable DMTOL EMTOL RMTOL NTTOL NRTOL RTTOL RRTOL Type F F F F F F F Default 0.0 0.0 0.0 0.0 0.0 0.0 0.0 Arc Length Optional Card. The contents of this card are ignored unless an arc-length method is activated (6 ≤ NSOLVR ≤ 9, or NSOLVR = 12 and ARCMTH = 3). Optional 3 1 2 3 4 5 6 7 8 Variable ARCCTL ARCDIR ARCLEN ARCMTH ARCDMP ARCPSI ARCALF ARCTIM Type Default I 0 I none F 0 I 1 I 2 F 0. F 0. F 0. Line Search Parameter Optional Card. Optional 4 1 2 3 4 5 6 7 8 Variable LSMTD LSDIR IRAD SRAD AWGT SRED Type Default I 4 I 2 F F F F 0.0 0.0 0.0 0.0 VARIABLE DESCRIPTION NSOLVR Solution method for implicit analysis: EQ.1: Linear EQ.12: Nonlinear with BFGS updates + optional arclength, (default) incorporating different line search and inte- gration schemes compared to solver 2. EQ.2: Nonlinear with BFGS updates (obsolete) VARIABLE DESCRIPTION EQ.3: Nonlinear with Broyden updates EQ.4: Nonlinear with DFP updates EQ.5: Nonlinear with Davidon updates EQ.6: Nonlinear with BFGS updates + arclength EQ.7: Nonlinear with Broyden updates + arclength EQ.8: Nonlinear with DFP updates + arclength EQ.9: Nonlinear with Davidon updates + arclength ILIMIT Iteration limit between automatic stiffness reformations MAXREF Stiffness reformation limit per time step. LT.0: If |MAXREF| matrix reformations occur convergence for that time step is forced, see REMARKS. DCTOL Displacement relative convergence tolerance ECTOL Energy relative convergence tolerance RCTOL Residual (force) relative convergence tolerance (DEFAULT = inactive) LSTOL Line search convergence tolerance ABSTOL Absolute convergence tolerance. LT.0: Convergence detected when the residual norm is less than –ABSTOL (Tip: To drive convergence based on – ABSTOL, set DCTOL and ECTOL to 1.0E-20) DNORM Displacement norm for convergence test EQ.1: Increment vs. displacement over current step EQ.2: Increment vs. total displacement (default) If DNORM.LT.0, this is to be interpreted as its absolute value, but activates reading of optional card 2b. DIVERG Divergence flag (force imbalance increase during equilibrium iterations) EQ.1: reform stiffness if divergence detected (default) VARIABLE DESCRIPTION EQ.2: ignore divergence ISTIF Initial stiffness formation flag EQ.1: reform stiffness at start of each step (default) EQ.n: reform stiffness at start of every “n”th step NLPRINT Nonlinear solver print flag EQ.0: no nonlinear iteration information printed (new v970 default) EQ.1: print iteration information to screen, message, d3hsp files EQ.2: print extra norm information (NLNORM = 1) EQ.3: same as 2, but also print information from line search NOTE: during execution, interactive commands can be used: response toggle NLPRINT between 0 and 1 toggle NLPRINT between 0 and 2 interactive command <ctrl-c> nlprint <ctrl-c> diagnostic <ctrl-c> information set NLPRINT = 2 for one iteration NLNORM Nonlinear convergence norm type, input an integer if zero or a positive number is used and float if a negative value is used LT.0: Same as 4, but rotational degrees of freedom are scaled appropriately with characteristic length |NLNORM| to account for units. See remarks. EQ.1: consider translational and rotational degrees of freedom EQ.2: consider translational degrees of freedom only (default) EQ.4: consider sum of translational and rotational degrees of freedom, i.e., no separate treatment. See remarks. D3ITCTL Control d3iter database. If nonzero, the search directions for the nonlinear implicit solution are written to the d3iter database. To reduce the size of the d3iter database the database is reset every n time steps where n = d3itctl. CPCHK Contact penetration check flag. This flag does not apply to mortar contacts. EQ.0: no contact penetration check is performed (default). VARIABLE DESCRIPTION DMTOL EMTOL RMTOL NTTOL NRTOL RTTOL RRTOL EQ.1: check for contact penetration during the nonlinear solution procedure. If such penetration is found modify the line search to prevent unnecessary penetration. Maximum displacement convergence tolerance, convergence is detected when the relative maximum nodal or rigid body displacement is less than this value Maximum energy convergence tolerance, convergence is detected when the relative maximum nodal or rigid body energy increment is less than this value is Maximum residual convergence detected when the relative maximum nodal or rigid body residual is less than this value tolerance, convergence translational convergence is Nodal detected when the absolute maximum nodal translational residual is less than this value tolerance, convergence Nodal rotational convergence tolerance, convergence is detected when the absolute maximum nodal rotational residual is less than this value Rigid body translational convergence tolerance, convergence is detected when the absolute maximum rigid body translational residual is less than this value Rigid body rotational convergence tolerance, convergence is detected when the absolute maximum rigid body rotational residual is less than this value ARCLEN Relative arc length size. See remarks below. LE.0.0: use automatic size, GT.0.0: use ARCLEN × (automatic step size). ARCMTH Arc length method EQ.1: Crisfield (default) EQ.2: Ramm EQ.3: Modified Crisfield (used with NSOLVR = 12 only) ARCDMP Arc length damping option VARIABLE DESCRIPTION EQ.2: off (default) EQ.1: on, oscillations in static solution are suppressed ARCPSI ARCALF Relative influence of load/time parameter in spherical arclength constraint, default value is 0 which corresponds to a cylindrical arclength constraint. Applies to ARCMTH = 3. Relative influence of predictor step direction for positioning of the arc center, default is 0 which means that the center is at the origin. Applies to ARCMTH = 3. ARCTIM Optional time when arclength method is initiated. Applies to ARCMTH = 3. LSMTD Line search convergence method: EQ.1: Energy method using only translational variables EQ.2: Residual method EQ.3: Energy method using both translational and rotational variables EQ.4: Energy method using sum of translational and rotational degrees of freedom (default), i.e., no separate treatment EQ.5: Same as 4, but account for residual norm growth to be extra conservative in step length EQ.6: Same as 5, but minimizes the residual norm whenever convenient. LSDIR Line search direction method: EQ.1: Search on all variables (traditional approach used in versions prior to 971) EQ.2: Search only on the independent (unconstrained) variables EQ.3: Use adaptive line search EQ.4: Use curved line search IRAD Normalized curvature factor for curved line search, where 0 indicates a straight line search and 1 indicates full curved line search. SRAD Radius of influence for determining curve in curved line search. VARIABLE DESCRIPTION For each independent node, all nodes within this radius are used for determining the curve. If 0, then all nodes connected to the same element as the independent node are used. AWGT SRED Adaptive line search weight factor between 0 and 1. A high value tends to restrict the motion of oscillating nodes during the implicit process. Initial step reduction between 0 and 1 for adaptive line search, use large number for conservative start in implicit procedure. Remarks: VARIABLE NSOLVR ILIMIT REMARKS If a linear analysis is selected, equilibrium checking and iterations are not performed. The Full Newton nonlinear solution method can be invoked by using the default BFGS solver, and selecting ILIMIT = 1 to form a new stiffness matrix every iteration. In the neighborhood of limit points the Newton based iteration schemes often fail. The arc length method of Riks and Wempner (combined here with the BFGS method) adds a constraint equation to limit the load step to a constant "arc length" in load-displacement space. This method is frequently used to solve snap through buckling problems. When applying the arc-length method, the curves that define the loading should contain only two points, and the first point should be at the origin (0,0). LS-DYNA will extrapolate, if necessary, to determine the load. In this way, time and load magnitude are related by a constant. It is possible that time can become negative in case of load reversal. The arc length method cannot be used in a dynamic analysis. In the default BFGS method, the global stiffness matrix is only reformed every ILIMIT iterations. Otherwise, an inexpensive stiffness update is applied. By setting ILIMIT = 1, a stiffness reformation is performed every iteration. This is equivalent to the Full Newton method (with line search). A higher value of ILIMIT (20-25) can reduce the number of stiffness matrix reformations and factorizations which may lead to a significant reduction in cost. Note that the storage requirements for VARIABLE REMARKS MAXREF DCTOL ECTOL RCTOL DMTOL, etc. implicit include storing 2 vectors per iteration. Large values of ILIMIT will cause substantial increase in storage requirements. The nonlinear equilibrium search will continue until the stiffness matrix has been reformed |MAXREF| times, with ILIMIT iterations between each reformation. If equilibrium has not been found and MAXREF > 0, control will be passed to the automatic time step controller if it is activated. If the automatic time step controller is not active error termination will result. When the auto time step controller is active, it is often efficient to choose MAXREF = 5 and try another stepsize quickly, rather than wasting too many iterations on a difficult step. When MAXREF < 0 and |MAXREF| matrix reformations have occurred convergence for the current time step is declared, with a warning, and the simulation moves to the next time step. This option should be used with caution as the results for that particular time step may be wrong. When the displacement norm ratio is reduced below DCTOL, this condition is satisfied. Smaller numbers lead to more accurate determination of equilibrium and, on the negative side, result in more iterations and higher costs. Use NLPRINT to display norm data each iteration. When the energy norm ratio is reduced below ECTOL, this condition is satisfied. Smaller numbers lead to more strict determination of equilibrium and, on the negative side, result in more iterations and higher costs. Use NLPRINT to display norm data each iteration. When the residual norm ratio is reduced below RCTOL, this condition is satisfied. Smaller numbers lead to more strict determination of equilibrium and, on the negative side, result in more iterations and higher costs. By default this convergence criterion is effectively disabled using RCTOL = 1.e10. Use NLPRINT to display norm data each iteration. For all nonzero values of the strict tolerance parameters in optional card 2b, the associated criterion must be satisfied in addition to the ones defined through DCTOL, ECTOL and RCTOL. These criteria are based on the maximum norm, which is regarded as stronger than the Euclidian norm used for the other parameters, and using them will likely result in higher VARIABLE REMARKS accuracy at the price of more iterations. For NLPRINT.GE.2 a table is listed in the message and d3hsp for each iteration, providing the values associated with all the criteria activated. The first three (DMTOL, EMTOL and RMTOL) of these extra parameters are unitless and honor the meaning of both DNORM and NLNORM. The last four (NTTOL, NRTOL, RTTOL and RRTOL) are to be given in units force, torque, force and torque, respectively, and the values used should account for the representative loads in the problem as well as the discretization size. A line search is performed on stiffening systems to guard against divergence of Newton-based nonlinear solvers. With the Full Newton method, it is sometimes helpful to define a large value (LSTOL = 9999.0) to effectively disable line search. When computing the displacement ratio, the norm of the incremental displacement vector is divided by the norm of “total” displacement. This “total” displacement may be either the total over the current step, or the total over the entire simulation. The latter tends to be more lax, and can be poor at the end of simulations where large motions develop. For these is DNORM = 1, and problems, an effective combination DCTOL = 0.01 or larger. By default, a new stiffness matrix is formed whenever divergence (growing out-of-balance force) is detected. This flag can be used to suppress this stiffness reformation. By default, a new stiffness matrix is formed at the start of every time step. Suppressing this stiffness reformation can decrease the cost of simulations which have many tiny steps that are mostly linear, such as transient dynamics. This flag controls printing of displacement and energy convergence measures during the nonlinear equilibrium search. If convergence difficulty occurs, this information is helpful in determining the problem. By default, only translational degrees of freedom are used in evaluating convergence norms. Use this flag to include rotational degrees of freedom, or to make additional data available for diagnosing convergence problems. LSTOL DNORM DIVERGE ISTIF NLPRINT NLNORM VARIABLE REMARKS This additional data includes the worst offending node and degree of freedom contributing to each norm. Rotational degrees of freedom can be considered independently from the translational degrees of freedom, meaning that two separate scalar products are used for evaluating norms, 〈𝐮, 𝐯〉t = 𝐮T𝐉t𝐯 and 〈𝐮, 𝐯〉r = 𝐮T𝐉r𝐯. Here 𝐉t and 𝐉r are diagonal matrices with ones on the diagonal to extract the translational and rotational degrees of the option NLNORM = 1, and the convergence criteria must be satisfied for both translational and rotational degrees of freedom simultaneously. freedom, respectively. This is Alternatively they can be included by defining the single scalar product 〈𝐮, 𝐯〉 = 〈𝐮, 𝐯〉t + 𝜆𝑢𝜆𝑣〈𝐮, 𝐯〉r, where 𝜆𝑢 and 𝜆𝑣 are scale factors to account for different units of the rotational degrees of freedom. For NLNORM = 4 these scale factors are equal to 1, but for NLNORM < 0 𝜆𝑢 is equal to |NLNORM| if u is a displacement vector and |NLNORM|−1 if it is a force vector, and the same goes for the pair 𝜆𝑣 and 𝐯. So |NLNORM| is a characteristic length that appropriately weighs translational and rotational degrees of freedom together. The arc length method can be controlled based on the displacement of a single node in the model. For example, in dome reversal problems the node at the center of the dome can be used. By default, the generalized arc length method is used, where the norm of the global displacement vector controls the solution. This includes all nodes. In many cases the arc length method has difficulty tracking the load displacement curve through critical regions. Using 0 < ARCLEN < 1 will reduce the step size to assist tracking the Use of load-displacement curve with more accuracy. ARCLEN < 1 will cause more steps to be taken. Suggested values are 1.0 (the default), 0.5, 0.25, and 0.10. Some static problems exhibit oscillatory response near instability points. This option numerically suppresses these oscillations, and may improve the convergence behavior of the post-buckling solution. ARCCTL ARCLEN ARCDMP LMSTD The default method for determining convergence of the nonlinear line search is to find the minimum of the energy. This VARIABLE REMARKS LSDIR IRAD / SRAD parameter allows choosing the energy on only the translational variables, energy of both the translational and rotational variables, or for minimizing the residual (forces). The effect of using a residual based line search is not always positive, sometimes it is too restrictive and stops convergence. However, it is a more conservative approach than using the energy based method since it explicitly controls the norm of the residual. It should not be seen as a better strategy than the energy method but as an alternative to try in cases when the default method seems to be working poorly. Line search methods 5 and 6 are conservative line search methods to be used for highly nonlinear problems, these should not be used as default but as final resorts to potentially resolve convergence issues. The rule of thumb is that the LSMTD = 5 is slow but robust and LSMTD = 6 is even slower but more robust. In Version 971 of LS-DYNA new line search options were added. The traditional approach (LSDIR = 1) computes the line search direction using all variables. The new (default) approach of LSIDR = 2 computes the line search direction only on the unconstrained variables. It has proven to be both robust and more efficient. We have also included two new approaches to try for problems where the default and traditional approach fail and the user is using Full Newton (ILIMIT = 1). See the next two remarks for more information on those methods. The parameters IRAD and SRAD are for the curved line search (LSDIR = 4). The first parameter is a switch (0 or 1) to invoke this line search, an intermediate value is interpreted as weighted combination of a straight and curved line search (the curvature radius is decreased with increasing IRAD). A value of unit is recommended in situations with rather smooth responses, e.g. springback and similar problems. Also, IRAD = 1 seems to work best with full Newton iterations. The SRAD parameter should be equal to 0 for most cases, this means that the search curve for a node is determined from the search direction of nodes connected to the same elements as that node. SRAD > 0 is interpreted as a radius of influence, meaning that the search curve for a node is determined from the search direction of nodes within a distance SRAD of this node. This option was introduced as an experiment to see if this had a smoothing and stabilizing effect. A value of 0.0 is VARIABLE REMARKS currently recommended. AWGT / SRED The parameters AWGT and SRED are for the adaptive line search. The intention is to improve robustness for problems that have tendencies to oscillate or diverge, indicated by the dnorm and enorm parameter outputs in the iterations (stdout). A value of 0.5 is recommended for AWGT as a starting point. With a nonzero value the motions of individual nodes are tracked. For nodes that are oscillating (going back and forth in space), the maximum step size for the next iteration is reduced in proportion to the parameter AWGT, and for nodes that are not oscillating but going nicely along a straight path, the maximum step size for the next iteration is increased in proportion to 1-AWGT. In test problems, the introduction of the adaptive line search has stabilized the implicit procedure in the sense that the dnorm and enorm values are more monotonically decreasing until convergence with virtually no oscillations. If a problem is still oscillating or diverging, the user should try to increase the AWGT parameter since this is a more restrictive approach but probably gives a slower convergence rate. An option for nasty problems is also to use SRED > 0 which is the initial step reduction factor (less than 1). This means that the initial step size is reduced by this value but the maximum step size will increase by an amount that is determined by the success in the iterative procedure, eventually it will reach unity. It can never decrease. Also here, it is intended to be used with full Newton method. *CONTROL_IMPLICIT_SOLVER_{OPTION} Available options include: <BLANK> DYN SPR Purpose: These optional cards apply to implicit calculations. The linear equation solver performs the CPU-intensive stiffness matrix inversion . The DYN option allows setting controls specifically for the dynamic relaxation phase. The SPR option allows setting controls specifically for the springback phase. Card 1 1 2 3 4 5 6 7 8 Variable LSOLVR LPRINT NEGEV ORDER DRCM DRCPRM AUTOSPC AUTOTOL Type I Default 4 I 0 I 2 I 0 I 4 F see below I 1 F see below Card 2 is optional. Card 2 1 2 3 4 5 6 7 8 Variable LCPACK MTXDMP Type Default I 2 I VARIABLE DESCRIPTION LSOLVR Linear equation solver method . EQ.4: SMP parallel multi-frontal sparse solver (default). EQ.5: SMP parallel multi-frontal sparse solver, double precision EQ.6: BCSLIB-EXT, direct, sparse, double precision EQ.10: iterative, best of currently available iterative methods EQ.11: iterative, Conjugate Gradient method EQ.12: iterative, CG with Jacobi preconditioner EQ.13: iterative, CG with Incomplete Choleski preconditioner EQ.14: iterative, Lanczos method EQ.15: iterative, Lanczos with Jacobi preconditioner EQ.16: iterative, Lanczos with Incomplete Choleski precondi- tioner LPRINT Linear solver print flag controls screen and message file output . EQ.0: no printing EQ.1: output summary statistics on memory, cpu requirements EQ.2: more statistics EQ.3: even more statistics and debug checking NOTE: during execution, use the interactive command "<ctrl- c> lprint" to toggle this print flag between 0 and 1. NEGEV Negative eigenvalue flag. Selects procedure when negative eigenvalues are detected during stiffness matrix inversion . EQ.1: stop, or retry step if auto step control is active EQ.2: print warning message, try to continue (default) ORDER Ordering option EQ.0: method set automatically by LS-DYNA EQ.1: MMD, Multiple Minimum Degree. EQ.2: Metis VARIABLE DRCM DESCRIPTION Drilling rotation constraint method for shells . EQ.1: add drilling stiffness (old Version 970 method) DRCPRM EQ.2: same as 4 below EQ.3: add no drilling stiffness EQ.4: add drilling stiffness (improved method) (default) Drilling rotation constraint parameter for shells. This parameter scales the drilling stiffness. For the old method (DRCM = 1) the default value of DRCPRM is 1.0 for linear analysis, 100.0 for nonlinear implicit analysis,; and either 1.E-12 or 1.E-8 for eigenvalue analysis depending on the shell element type. For eigenvalue analysis, the input value for DRCPRM is ignored. For the improved method (default, DRCM = 4), the default value of DRCPRM is as described above for the old method except default DRCPRM is 1.0 for nonlinear implicit analysis. AUTOSPC Automatic Constraint Scan flag EQ.1: scan the assembled stiffness matrix for unconstrained, unattached degrees of freedom. Generate additional constraints as necessary to avoid negative eigenvalues. looking EQ.2: do not add constraints. AUTOTOL AUTOSPC tolerance. The test for singularity is the ratio of the smallest singular value and the largest singular value. If this ratio is less than AUTOTOL, then the triple of columns are declared singular and a constraint is generated. Default value in single precision is 10−4 and in double precision, 10−8. LCPACK Matrix assembly package. MTXDMP EQ.2: Use v970’s LCPACK (default, only available option in 971) EQ.3: Same as 2, but incorporates a non-symmetric linear solver, see remark for LCPACK. Matrix and right-hand-side dumping. LS-DYNA has the option of dumping the globally assembled stiffness matrix and right- hand-side vectors files in Harwell-Boeing sparse matrix format. Such output may be useful for comparing to other linear equation solution packages. VARIABLE DESCRIPTION EQ.0: No dumping GT.0: Dump all matrices and right-hand-side vectors every MTXDMP time steps. Output is written as ASCII text and the iinvolved filenames are of the following form: K_xxxx_yyy.mtx.rb This file contains the stiffness matrix at step xxxx, it- eration yyy. M_xxxx_yyy.mtx.rb This file contains the mass matrix at step xxxx, itera- tion. Only for eigenvalue analysis. MW_xxxx_yyy.mtx.rb This file contains the damping matrix at step xxxx, it- eration. Only for simulations with damping. K_xxxx_yyy_zzz.rhs.rb This file contains the right hand side at step xxxx, it- eration yyy, where yyy is the iteration at which a stiffness matrix is formed; zzz is the cumulative itera- tion number for the step. The values of yyy and zzz don’t always coincide because the stiffness matrix is not necessarily reformed every iteration. Node_Data_xxxx_yyy This file maps stiffness matrix to nodes and provides nodal coordinates. LT.0: Like positive values of MTXDMP but dumped data is binary. EQ.|9999|: Simulation is terminated after dumping matrices and right hand side prior to factorization. Remarks: VARIABLE LSOLVR REMARKS The linear solver is used to compute the inverse of the global stiffness matrix, which is a costly procedure both in memory and cpu time. Direct solvers apply Gaussian elimination, while iterative solvers successively improve “guesses” at the correct solution. Iterative solvers require far less memory than direct VARIABLE REMARKS solvers, but may suffer from convergence problems. Generally, iterative solvers are poor for automotive applications, but can be superior for large brick element soil models in civil engineering. Solvers 5 and 6 promote the global matrix to double precision before factoring to reduce numerical truncation error. Solvers 4 and 5 are equivalent if a double precision executable is used. Solver 6 is the direct linear equation solver from BCSLIB-EXT, Boeing's Extreme Mathematical Library. This option should be used whenever the factorization is too large to fit into memory. It has extensive capabilities for out-of-core solution and can solve larger problems than any of the other direct factorization methods. Solver 6 also includes a sophisticated pivoting strategy which can be superior for nearly singular matrices. Solver 5 is the only option supported in MPP. LPRINT NEGEV the storage timing and Select printing of information (LPRINT = 1) if you are comparing performance of linear equation solvers, or if you are running out of memory for large models. Minimum memory requirements for in-core and out-of- core solution are printed. This flag can also be toggled using sense switch "<ctrl-c> lprint". For best performance, increase available memory using “memory=“ on the command line until an IN- CORE solution is indicated. When using solver option 6, LPRINT = 2 and 3 will cause increased printed output of statistics and performance information. Negative eigenvalues result from underconstrained models (rigid body modes), severely deformed elements, or non-physical material properties. This flag allows control to be passed directly to the automatic time step controller when negative eigenvalues are detected. Otherwise, significant numerical roundoff error is likely to occur during factorization, and equilibrium iterations may fail . ORDER DRCPRM LCPACK *CONTROL_IMPLICIT_SOLVER REMARKS The system of linear equations is reordered to optimize the sparsity of the factorization when using direct methods. Metis is a ordering method from University of Minnesota which is very effective for larger problems and for 3D solid problems, but also very expensive. MMD is inexpensive, but may not produce an optimum reordering, leading to higher cost during numeric factorization. MMD is usually best for smaller problems (less than 100,000 degrees of freedom). Reordering cost is included in the symbolic factorization phase of the linear solver (LSPRINT ≥ 1). For large models, if this cost exceeds 20% of the numeric factorization cost, it may be more efficient to select the MMD method. Note that the values of LPRINT and ORDER also affect the eigensolution software. That is LPRINT and ORDER from this keyword card is applicable to eigensolution. To avoid a singular stiffness matrix in implicit analysis of flat shell topologies, some constraint on the drilling degree of freedom is needed. The default method of applying this constraint, DRCPRM = 4, adds the consistent force vector for consistency and improved convergence as compared to the old method, DRCPRM = 1. In explicit analysis, an unconstrained drilling degree of freedom is usually not a concern since a stiffness matrix is not used. However, special situations may arise in which the user wishes to include additional resisting rotational force in the drilling degree of freedom for improved robustness and/or accuracy. To activate the consistent drilling constraint in explicit analysis, use the input variables DRCPSID and DRCPRM for *CONTROL_SHELL. Certain features may break the symmetry of the stiffness matrix. Unless LCPACK is set to 3 these contributions are suppressed or symmetrized by the default symmetric linear solver. However, when LCPACK is set to 3 a more general linear solver lifting the symmetry requirement is used. The solver for non-symmetric matrices is more computationally expensive. Keywords implemented are listed below: for which the non-symmetric contribution is *CONTACT_..._MORTAR: VARIABLE REMARKS The mortar contact accounts for frictional non-symmetry in the resulting tangent stiffness matrix, the effects on convergence characteristics have not yet shown to be significant. *LOAD_SEGMENT_NONUNIFORM: The non-symmetric contribution may be significant for the follower load option, LCID < 0. *LOAD_SEGMENT_SET_NONUNIFORM: The non-symmetric contribution may be significant for the follower load option, LCID < 0. *MAT_FABRIC_MAP: This stress map fabric model accounts for non-symmetry in the material tangent modulus, representing the non- linear Poisson effect due to complex interaction of yarns. *SECTION_SHELL, *SECTION_SOLID: User defined resultant elements (ELFORM = 101, 102, 103, 104, 105 with NIP=0) support the assembly and solution of non-symmetric element matrices. *SECTION_BEAM: Belytschko-Schwer beam geometric stiffness contribution is supported. (ELFORM=2) nonsymmetric *CONTROL_IMPLICIT_STABILIZATION_{OPTION} Available options include: <BLANK> DYN SPR Purpose: This optional card applies to implicit calculations. Artificial stabilization is required for multi-step unloading in implicit springback analysis . The DYN option allows setting controls specifically for the dynamic relaxation phase. The SPR option allows setting controls specifically for the springback phase. Card 1 1 2 3 4 5 6 7 8 Variable IAS SCALE TSTART TEND Type I F F F Default 2 1.0 see below see below VARIABLE DESCRIPTION IAS Artificial Stabilization flag EQ.1: active EQ.2: inactive (default) SCALE Scale factor for artificial stabilization. For flexible parts with large springback, like outer body panels, a value of 0.001 may be required. EQ.-n: curve ID = n gives SCALE as a function of time TSTART Start time. (Default: immediately upon entering implicit mode) TEND End time. (Default: termination time) Remarks: Artificial stabilization allows springback to occur over several steps. This is often necessary to obtain convergence during equilibrium iterations on problems with large springback deformation. Stabilization is introduced at the start time TSTART, and slowly removed as the end time TEND is approached. Intermediate results are not accurate representations of the fully unloaded state. The end time TEND must be reached exactly for total springback to be predicted accurately. VARIABLE IAS SCALE REMARKS The default for IAS depends on the analysis type in *CONTROL_- IMPLICIT_GENERAL. For “seamless” springback analysis, automatic time step control and artificial stabilization are activated by default. Otherwise, IAS is inactive by default. This is a penalty scale factor similar to that used in contact interfaces. If modified, it should be changed in order-of- magnitude increments at first. Large values suppress springback deformation until very near the termination time, making convergence during the first few steps easy. Small values may not stabilize the solution enough to allow equilibrium iterations to converge. *CONTROL_IMPLICIT_STATIC_CONDENSATION_{OPTION} Available options include: <BLANK> BINARY Purpose: Request static condensation of a part to build a reduced linearized model for later computation with *ELEMENT_DIRECT_MATRIX_INPUT. Optionally the analysis can continue using the linearization for the current analysis. Card 1 1 2 3 4 5 6 7 8 Variable SC_FLAG SC_NSID SC_PSID SE_MASS SE_STIFF SE_INERT I 0 2 I 0 3 Type Default I 0 Card 2 1 Variable Type C C C 4 5 6 7 8 SE_FILENAME A80 VARIABLE DESCRIPTION SC_FLAG Static Condensation Control Flag EQ.0: no static condensation will be performed EQ.1: create superelement representation based on static condensation. EQ.2: use static condensation to build a linearized representa- tion for a part and use that linearized representation in the following analysis. SC_NSID Node set ID for nodes to be preserved in the static condensation procedure. Required when SC_FLAG = 1. VARIABLE SC_PSID SE_MASS SE_STIFF SE_INERT DESCRIPTION Part set ID for parts to be included in the static condensation procedure. When SC_FLAG = 1, SC_PSID can be used to specify a subset of the model with the default being the entire model. When SC_FLAG = 2, SC_PSID is required. SC_PSID = 0 implies that the entire model is condensed. Name of the superelement mass matrix. If left blank it is not generated. Name of the superelement stiffness matrix. If left blank it is not generated. Name of the superelement inertia matrix, required for gravity loading applications of the superelement. If left blank it is not generated. SE_FILENAME If any of SE_MASS, SE_STIFF, or SE_INERT is blank then the second line is required and contains the file name for the superelement. Remarks: To use this feature, an implicit analysis must be requested using IMFLAG = 1 on *CON- TROL_IMPLICIT_GENERAL, and a non-zero termination time must be specified on *CONTROL_TERMINATION. A double precision version of LS-DYNA should be used for best accuracy. The superelement model is written to file SE_FILENAME. Static condenstation is the reduction of the global stiffness and mass matrices to a specified sets of rows and columns associated with the nodes in the node set SC_NSID. The first and second node set attribute parameters can be optionally used to restrict the translational and rotational degrees of freedom for which modes are requested, respectively, according to the following syntax: Node set attribute parameters DA1 and A1: translational degree of freedom codes Node set attribute parameters DA2 and A2: rotational degree of freedom codes Code 0 1 2 3 4 5 6 7 Modes Computed X degree of freedom only Y degree of freedom only Z degree of freedom only X, Y degrees of freedom only Y, Z degrees of freedom only X, Z degrees of freedom only X, Y, Z degrees of freedom Setting both node set attributes to zero is equivalent to setting both node set attributes to 7 (X, Y, and Z for translational and rotational degrees of freedom). If one node set attribute is nonzero (codes 1 to 7) and the other node set attribute is zero, then the zero attribute means NO degrees of freedom are considered. For example, if DA1 = 2 and DA2 = 0, then only the Y-translational degree of freedom modes are calculated. The user can create the superelement representation of the reduced model by specifying the SE_MASS, SE_STIFF, SE_INERT and SE_FILENAME fields. This implementation does not include SE_DAMP. The file, by default is written in the Nastran DMIG file format and can be used as input to *ELEMENT_DIRECT_MATRIX_INPUT. The keyword option BINARY can be used to create a binary representation for the superelement which can be used with *ELEMENT_DIRECT_MATRIX_INPUT_BINARY to reduce the file size. Static Condensation is equivalent to using only constraint modes with *CONTROL_IM- PLICIT_MODES. Static Condensation does have the ability to continue the analysis using the linear representation for a part set. *CONTROL_IMPLICIT_TERMINATION Purpose: Specify termination criteria for implicit transient simulations. Card 1 1 2 3 4 5 6 7 8 Variable DELTAU DELTA1 KETOL IETOL TETOL NSTEP Type F F F F F Default 0.0 0.0 0.0 0.0 0.0 I 3 VARIABLE DELTAU DESCRIPTION Terminate based on relative total displacement in the Euclidean norm. GT.0.0: terminate when displacement in the Euclidean norm for last time step relative to the total displacement in the Euclidean norm is less than DELTAU. DELTA1 Terminate based on relative total displacement in the max norm. GT.0.0: terminate when displacement in the max norm for last time step relative to the total displacement in the max norm is less than DELTAU. KETOL Terminate based on kinetic energy GT.0.0: terminate when kinetic energy drops below KETOL for NSTEP consecutive implicit time steps. IETOL Terminate based on internal energy GT.0.0: terminate when internal energy drops below IETOL for NSTEP consecutive implicit time steps. TETOL Terminate based on total energy GT.0.0: terminate when total energy drops below TETOL for NSTEP consecutive implicit time steps. NSTEP Number of steps used in the early termination tests for kinetic, internal, and total energy. *CONTROL_IMPLICIT_TERMINATION For some implicit applications it is useful to terminate when there is no change in displacement or low energy. This keyword provides the ability to specify such a stopping criterias to terminate the simulation prior to ENDTIM. *CONTROL Purpose: Define global control parameters for material model related properties. Card 1 1 2 3 4 5 6 7 8 Variable MAEF Type Default I 0 VARIABLE DESCRIPTION MAEF Failure options: EQ.0: all *MAT_ADD_EROSION definitions are active. EQ.1: switch off all *MAT_ADD_EROSION definitions globally. This feature is useful for larger models where removing the *MAT_ADD_EROSION cards is incon- vient. *CONTROL_MPP Purpose: Set control parameters for MPP specific features. *CONTROL_MPP_CONTACT_GROUPABLE *CONTROL_MPP_DECOMPOSITION_ARRANGE_PARTS *CONTROL_MPP_DECOMPOSITION_AUTOMATIC *CONTROL_MPP_DECOMPOSITION_BAGREF *CONTROL_MPP_DECOMPOSITION_CHECK_SPEED *CONTROL_MPP_DECOMPOSITION_CONTACT_DISTRIBUTE *CONTROL_MPP_DECOMPOSITION_CONTACT_ISOLATE *CONTROL_MPP_DECOMPOSITION_DISABLE_UNREF_CURVES *CONTROL_MPP_DECOMPOSITION_DISTRIBUTE_ALE_ELEMENTS *CONTROL_MPP_DECOMPOSITION_DISTRIBUTE_SALE_ELEMENTS *CONTROL_MPP_DECOMPOSITION_DISTRIBUTE_SPH_ELEMENTS *CONTROL_MPP_DECOMPOSITION_ELCOST *CONTROL_MPP_DECOMPOSITION_FILE *CONTROL_MPP_DECOMPOSITION_METHOD *CONTROL_MPP_DECOMPOSITION_NUMPROC *CONTROL_MPP_DECOMPOSITION_OUTDECOMP *CONTROL_MPP_DECOMPOSITION_PARTS_DISTRIBUTE *CONTROL_MPP_DECOMPOSITION_PARTSET_DISTRIBUTE *CONTROL_MPP_DECOMPOSITION_RCBLOG *CONTROL_MPP_DECOMPOSITION_SCALE_CONTACT_COST *CONTROL_MPP_DECOMPOSITION_SCALE_FACTOR_SPH *CONTROL_MPP_DECOMPOSITION_SHOW *CONTROL_MPP_DECOMPOSITION_TRANSFORMATION *CONTROL_MPP_IO_LSTC_REDUCE *CONTROL_MPP_IO_NOBEAMOUT *CONTROL_MPP_IO_NOD3DUMP *CONTROL_MPP_IO_NODUMP *CONTROL_MPP_IO_NOFAIL *CONTROL_MPP_IO_NOFULL *CONTROL_MPP_IO_SWAPBYTES *CONTROL_MPP_MATERIAL_MODEL_DRIVER *CONTROL_MPP_PFILE *CONTROL_MPP_CONTACT_GROUPABLE Purpose: Allow for global specification that the GROUPABLE algorithm should be enabled/disabled for contacts when running MPP. Card 1 1 2 3 4 5 6 7 8 Variable GRP Type I Default none VARIABLE GRP DESCRIPTION The sum of these available options (in any combination that makes sense): 1: Turn on GROUPABLE for all non-tied contacts 2: Turn on GROUPABLE for all tied contacts 4: Turn off GROUPABLE for all non-tied contacts 8: Turn off GROUPABLE for all tied contacts Remarks: The GROUPABLE algorithm is an alternate MPP communication algorithm for SIN- GLE_SURFACE, NODE_TO_SURFACE, and SURFACE_TO_SURFACE contacts. This algorithm does not support all contact options, including SOFT = 2, as of yet, and is still under development. It can be significantly faster and scale better than the normal algorithm when there are more than two or three applicable contact types defined in the model. Its intent is to speed up the contact processing but not to change the behavior of the contact. This keyword will override any setting of the GRPABLE parameter on the *CON- TACT_…_MPP card, and is intended as a way to quickly experiment with this feature. The equivalent pfile option is “contact { groupable GRP }” where GRP is an integer as described above. *CONTROL_MPP_DECOMPOSITION_ARRANGE_PARTS_OPTION Purpose: Allow users to distribute certain part(s) to all processors or to isolate certain part(s) in a single processor. This keyword supports multiple entries. Each entry is be processed as a separate region for decomposition. When this keyword is part of an included file and the LOCAL option is given, the decomposition will be done in the coordinate system of the included file, which may be different from the global system, if the file is included using the *INCLUDE_TRANS- FORM keyword. Card 1 Variable 1 ID 2 3 4 5 6 7 8 TYPE NPROC FRSTP Type I I I I Default none none None None VARIABLE DESCRIPTION ID TYPE Part ID/Part set ID EQ.0: Part ID to be distributed to all processors EQ.1: Part Set ID to be distributed to all processors EQ.10: Part ID to be lumped into one processor EQ.11: Part Set ID to be lumped into one processor. NPROC Used only for TYPE equal to 0 or 1. Evenly distributed Part ID/Part set ID to NPROC of processors. FRSTP Used only for TYPE equal to 0 or 1. Starting MPP rank ID. Remarks: There is no equivalent option under pfile. *CONTROL_MPP_DECOMPOSITION_AUTOMATIC Purpose: Instructs the program to apply a simple heuristic to try to determine the proper decomposition for the simulation. There are no input parameters. The existence of this keyword triggers the automated decomposition. This option should not be used if there is more than one occurrence of any of the following options in the model: *INITIAL_VELOCITY *CHANGE_VELOCITY *BOUNDARY_PRESCRIBED_MOTION And the following control card must not be used: *CONTROL_MPP_DECOMPOSITION_TRANSFORMATION For the general case, it is recommended that you specify the proper decomposition using *CONTROL_MPP_DECOMPOSITION_TRANSFORMATION instead. the command *CONTROL_MPP_DECOMPOSITION_BAGREF Purpose: With this card LS-DYNA performs decomposition according to the airbag’s reference geometry, rather than the folded geometry. Other than BAGID values this card takes no input parameters. The initial geometry may lead to a poor decomposition once the bag is deployed. This option will improve load balancing for the fully deployed geometry. Optional card(s) for selected reference geometry ID Card 1 1 2 3 4 5 6 7 8 Variable BAGID1 BAGID2 BAGID3 BAGID4 BAGID5 BAGID6 BAGID7 BAGID8 Type I I I I I I I I Default none none none none none none none none VARIABLE BAGIDi DESCRIPTION ID defined *AIRBAG_SHELL_REFERENCE_GEOMETRY_ID in *AIRBAG_REFERENCE_GEOMETRY_ID or Bags specified in the optional cards will be decomposed based on the reference geometry. If there is no card given, all bags will be decomposed by their reference geometry. Remarks: Command in partition file (pfile): BAGREF. The option for selecting particular airbags is only available when using keyword input. *CONTROL_MPP_DECOMPOSITION_CHECK_SPEED Purpose: Modifies the decomposition depending on the relative speed of the processors involved. There are no input parameters. Use of this keyword activates a short floating point timing routine to be executed on each processor. The information gathered is used during the decomposition, with faster processors being given a relatively larger portion of the problem. This option is not recommended on homogeneous systems. *CONTROL_MPP_DECOMPOSITION_CONTACT_DISTRIBUTE_OPTION Purpose: Ensures that the indicated contact interfaces are distributed across all processors, which can lead to better load balance for large contact interfaces. If this appears in an included file and the LOCAL option is given, the decomposition will be done in the coordinate system of the included file, which may be different from the global system if the file is included via *INCLUDE_TRANSFORM. Card 1 1 Variable ID1 2 ID2 3 ID3 4 ID4 5 ID5 6 7 8 Type I I I I I Default none none none none none DESCRIPTION First contact interface ID to distribute. If no contact ID's are specified, the number given here corresponds to the order of the interfaces as they appear in the input, with the first being 1. Remaining interfaces ID's to distribute. VARIABLE ID1 ID2, ID3, ID4, ID5 Remarks: Up to 5 contact interface ID's can be specified. The decomposition is modified as follows: First, all the elements involved in the first contact interface are decomposed across all the processors. Then all the elements involved in the second contact interface (excluding any already assigned to processors) are distributed, and so on. After all the contact interfaces given are processed, the rest of the input is decomposed in the normal manner. This will result in each processor having possibly several disjoint portions of the input assigned to it, which will increase communications somewhat. However, this can be offset by improved load balance in the contact. It is generally recommended that at most one or two interfaces be specified, and then only if they are of substantial size relative to the whole problem. *CONTROL_MPP_DECOMPOSITION_CONTACT_ISOLATE Purpose: Ensures that the indicated contact interfaces are isolated on a single processor, which can lead to decreased communication. Card 1 1 Variable ID1 2 ID2 3 ID3 4 ID4 5 ID5 6 7 8 Type I I I I I Default none none none none none DESCRIPTION First contact interface ID to isolate. If no contact ID's are specified, the number given here corresponds to the order of the interfaces as they appear in the input, with the first being 1. Remaining interfaces ID's to isolate. VARIABLE ID1 ID2, ID3, ID4, ID5 Remarks: Up to 5 contact interfaces can be specified. The decomposition is modified as follows: First, all the elements involved in the first contact interface ID are assigned to the first processor. Then all the elements involved in the second contact interface ID (excluding any already assigned to processors) are assigned to the next processor, and so on. After all the contact interfaces given are processed, the rest of the input is decomposed in the normal manner. This will result in each of the interfaces being processed on a single processor. For small contact interfaces this can result in better parallelism and decreased communication. Purpose: Disable unreferenced time dependent load curves for the following keyword. *BOUNDARY_PRESCRIBED_MOTION_NODE *LOAD_NODE *LOAD_SHELL_ELEMENT *LOAD_THERMAL_VARIABLE_NODE The details of this operation are reported in each processor’s scratch “scr####” file. This will skip the curve evaluation on each cycle, and improve the parallel efficiency. Remarks: Command in partition file (pfile): DUNREFLC. *CONTROL_MPP_DECOMPOSITION_DISTRIBUTE_ALE_ELEMENTS Purpose: Ensures ALE elements are evenly distributed to all processors There are no input parameters and the card below is optional. ALE elements usually have higher computational cost than other type of elements and it is better to distribute them to all CPU for better load balance. The existence of this keyword causes DYNA/MPP to extract ALE parts from input and then evenly distributed to all processors. The card is optional Card 1 1 2 3 4 5 6 7 8 Variable OVERLAP Type I Default none VARIABLE OVERLAP DESCRIPTION For FSI models where structures are inside ALE meshes , decompose structure and ALE domains together instead of first the structure and then ALE . Set type: EQ.0: Off EQ.1: On Remarks: 1. Command in partition file (pfile): ALEDIST. 2. Most of the processors will have to deal with MPP subdomains from the structure and ALE meshes: a portion of the ALE computational domain and a portion of the structure meshes. The default decomposition (first divide the structures, then ALE) does not always overlap these subdomains. The more they overlap, the lesser the MPP communications in the coupling cost. Cutting the ALE and structure meshes together allows their MPP subdomains to be as inclusive as possible. *CONTROL_MPP_DECOMPOSITION_DISTRIBUTE_SPH_ELEMENTS Purpose: Ensures SPH elements are evenly distributed to all processors There are no input parameters. SPH elements usually have higher computational cost than other type of elements and it is better to distribute them to all CPU for better load balance. The existence of this keyword causes DYNA/MPP to extract SPH parts from input and then evenly distributed to all processors. Remarks: Command in partition file (pfile): SPHDIST. *CONTROL_MPP_DECOMPOSITION_ELCOST Purpose: Instructs the program to use a hardware specific element cost weighting for the decomposition Card 1 1 2 3 4 5 6 7 8 Variable ITYPE Type I Default none VARIABLE DESCRIPTION ITYPE Hardware specific cost profile. EQ.1: Fujitsu PrimePower EQ.2: Intel IA 64, AMD Opteron EQ.3: Intel Xeon 64 EQ.4: General profile Remarks: Command in partition file (pfile): elcost itype. *CONTROL_MPP_DECOMPOSITION_FILE Purpose: Allow for pre-decomposition and a subsequent run or runs without having to do the decomposition. Card 1 1 2 3 4 5 6 7 8 Variable Type Default NAME A80 none VARIABLE DESCRIPTION NAME Name of a file containing (or to contain) a decomposition record. Remarks: If the indicated file does not exist, it is created with a copy of the decomposition information from this run. If the file exists, it is read and the decomposition steps can be skipped. The original run that created the file must be for a number of processors that is a multiple of the number of processors currently being used. Thus, a problem can be decomposed once for, say, 48 processors. Subsequent runs are then possible on any number that divides 48: 1, 2, 3, 4, 6, etc. Since the decomposition phase generally requires more memory than execution, this allows large models to be decomposed on one system and run on another (provided the systems have compatible binary formats). The file extension “.pre” is added automatically. *CONTROL_MPP_DECOMPOSITION_METHOD Purpose: Specify the decomposition method to use. Card 1 1 2 3 4 5 6 7 8 Variable Type Default VARIABLE NAME NAME A80 RCB DESCRIPTION Name of the decomposition method to use. There are currently two options: EQ.“RCB”: recursive coordinate bisection EQ.“GREEDY”: a simple heuristic method In almost all cases the RCB method is superior and should be used. *CONTROL_MPP_DECOMPOSITION_NUMPROC Purpose: Specify the number of processors for decomposition. 2 3 4 5 6 7 8 Card 1 Variable Type 1 N I Default none VARIABLE DESCRIPTION N Number of processors for decomposition. Remarks: This is used in conjunction with the CONTROL_MPP_DECOMPOSITION_FILE command to allow for later runs on different numbers of processors. By default, the decomposition is performed for the number of processors currently being used. However, a different value can be specified here. If N > 1 and only one processor is currently being used, the decomposition is done and then the program terminates. If N is not a multiple of the current number of processors, then it is ignored the execution proceeds with the current number of processors. Otherwise, the decomposition is performed for N processors, and the execution continues using the current number of processors. *CONTROL_MPP_DECOMPOSITION_OUTDECOMP Purpose: Instructs the program to output element's ownership data to file for post- processor to show state data from different processors Card 1 1 2 3 4 5 6 7 8 Variable TYPE Type I Default none VARIABLE DESCRIPTION ITYPE Sets the format for the output file. EQ.1: database in LS-PrePost format: decomp_parts.lsprepost. EQ.2: database in animator format: decomp_parts.ses Remarks: Command in partition file (pfile): OUTDECOMP ITYPE. When ITYPE is set to 1, the elements assigned to any particular core can be viewed and animated by LS-PrePost by (1) reading the d3plot data, and then (2) selecting Models > Views > MPP > Load > decomp_parts.lsprepost. *CONTROL_MPP_DECOMPOSITION_PARTS_DISTRIBUTE_OPTION Purpose: Distribute the parts given in this option to all processors before the decomposition for the rest of the model is performed. If this appears in an included file and the LOCAL option is given, the decomposition will be done in the coordinate system of the included file, which may be different from the global system if the file is included via *INCLUDE_TRANSFORM. Card 1 1 Variable ID1 2 ID2 3 ID3 4 ID4 5 ID5 6 ID6 7 ID7 8 ID8 Type I I I I I I I I Default none none none none none none none none VARIABLE ID1, ID2, ID3, … DESCRIPTION For each ID: GT.0: ID is a part number. LT.0: –ID is a part set number. All parts defined in this card will be treated as a single region to be decomposed. Remarks: Up to 16 parts/part sets can be specified. The decomposition is modified as follows: the elements involved in the given parts are put into a separate domain from rest of the model and then distributed to all processors to balance their computational cost. Then the remainder of the model will be distributed in the usual way. This is equivalent to the pfile command (for example, if ID1-ID3 are part ids and ID4- ID6 are partset ids): decomp { region { parts ID1 ID2 ID3 or partsets ID4 ID5 ID6 } } (the partset ids are positive when used in the pfile). *CONTROL_MPP_DECOMPOSITION_PARTSET_DISTRIBUTE_OPTION Purpose: Distribute the part sets given in this option to all processors before the decomposition for the remainder of the model is performed. If this appears in an included file and the LOCAL option is given, the decomposition will be done in the coordinate system of the included file, which may be different from the global system if the file is included via *INCLUDE_TRANSFORM. Card 1 1 Variable ID1 2 ID2 3 ID3 4 ID4 5 ID5 6 ID6 7 ID7 8 ID8 Type I I I I I I I I Default none none none none none none none none DESCRIPTION Partset ID to be distributed.. All parts in ID1 will be shared across all processors. Then all parts in ID2 will be distributed, and so on.. VARIABLE ID1, ID2, ID3, … Remarks: Any number of part sets can be specified. Each part set is distributed across all processors, in the order given. The order may be significant, in particular, if a part ID is in more than one set. Distribution of these parts is done before any decomposition specifications given in the pfile. *CONTROL_MPP_DECOMPOSITION_RCBLOG Purpose: Causes the program to record decomposition information in the indicated file, for use in subsequent analyses. Card 1 1 2 3 4 5 6 7 8 FILENAME A80 none DESCRIPTION Name of output file where decomposition history will be recorded. This file can be used as the pfile for later analyses. Variable Type Default VARIABLE FILENAME Remarks: Command in parallel option file (pfile): rcblog filename. *CONTROL_MPP_DECOMPOSITION_SCALE_CONTACT_COST Purpose: Instructs the program to apply a scale factor to the list of contacts to change the partition weight for the decomposition. Card 1 Variable 1 SF 2 ID1 3 ID2 4 ID3 5 ID4 6 ID5 7 ID6 8 ID7 Type F I I I I I I I Default none none none none none none none none VARIABLE DESCRIPTION SF Scale factor for the contact segments listed in the interface ID. ID1, ID2, … interfaces ID's to be considered for scaling. Include second card if necessary. Remarks: Up to 15 contact interfaces ID can be specified. The decomposition is modified by applying this scale factor to the default computational cost of elements for the given contact interface ID. Command in partition file (pfile): CTCOST ID1, ID2, …, SF. *CONTROL_MPP_DECOMPOSITION_SCALE_FACTOR_SPH Purpose: Instructs the program to apply a scale factor to SPH elements to change the partition weight for the decomposition. 2 3 4 5 6 7 8 Card 1 Variable 1 SF Type F Default none VARIABLE DESCRIPTION SF Scale factor Remarks: Command in partition file (pfile): SPHSF SF. *CONTROL_MPP_DECOMPOSITION_SHOW Purpose: The keyword writes the final decomposition to the d3plot database. There are no input parameters. This keyword causes MPP LS-DYNA to terminate immediately after the decomposition phase without performing an analysis. The resulting d3plot database is designed to allow visualization of the decomposition by making each part correspond to the group of solids, shells, beams, thick shells, or SPH particles assigned to a particular processor. For example, in a model that includes various element types including solids, part 1 corresponds to the solid elements assigned to processor 1, part 2 corresponds to the solid elements assigned to processor 2, and so on. This command can be used in conjunction with the *CONTROL_MPP_DECOMPOSI- TION_NUMPROC command to run on one processor and produce a d3plot file to visualize the resulting decomposition for the number of processors specified in *CON- TROL_MPP_DECOMPOSITION_NUMPROC. *CONTROL_MPP_DECOMPOSITION_TRANSFORMATION Purpose: Specifies transformations to apply to modify the decomposition. There are 10 different kinds of decomposition transformations available. For a detailed description of each, see Appendix O the LS-DYNA MPP user guide. The data cards for this keyword consist of transformation operations. Each operation, depending on its type, involves either one or two additional cards. The input deck may include an arbitrary number of transformations with the next keyword, “*,” card terminating this input. Transformation Card 1. For each transformation this card is required. Card 1 1 Variable TYPE 2 V1 Type A10 F 3 V2 F 4 V3 F 5 V4 F 6 V5 F 7 V6 F 8 Default none 0.0 0.0 0.0 0.0 0.0 0.0 Transformation Card 2. Additional card for TYPE set to one of VEC3, C2R, S2R, MAT. 4 5 6 7 8 Card 2 Variable 1 V7 Type F 2 V8 F 3 V9 F Default 0.0 0.0 0.0 VARIABLE TYPE DESCRIPTION Which transformation to apply. The allowed values are RX, RY, RZ, SX, SY, SZ, VEC3, C2R, S2R, and MAT. VARIABLE DESCRIPTION V1 - V9 For type set to either RX, RY, RZ, SX, SY, or SZ: The parameter V1 gives either the angle of rotation (RX, RY, RZ) or the magnitude for the scaling (SX, SY, SZ). The remaining parameters are ignored. For type set to either VEC3, C2R, S2R, or MAT: All parameters are used. See the appendix for the “pfile.” *CONTROL_MPP_IO_LSTC_REDUCE Purpose: Use LSTC's own reduce routine to get consistent summation of floating point data among processors. There are no input parameters. Remarks: Command in partition file (pfile): lstc_reduce. *CONTROL_MPP_IO_NOBEAMOUT Purpose: Suppress beam, shell, and solid element failure messages in the d3hsp and message files. There are no parameters for this keyword. Remarks: Command in parallel option file (pfile): nobeamout. *CONTROL_MPP_IO_NOD3DUMP Purpose: Suppresses the output of all dump files. There are no input parameters. The existence of this keyword causes the d3dump and runrsf file output routines to be skipped. *CONTROL_MPP_IO_NODUMP Purpose: Suppresses the output of all dump files and full deck restart files. There are no input parameters. The existence of this keyword causes the d3dump and runrsf file output routines to be skipped. It also suppresses output of the full deck restart file d3full. *CONTROL Purpose: Turn off failed element checking in MPP contact. If you know that no elements will fail, or that any such failure will not impact any of the contact calculations, turning on this option can increase the efficiency of the contact routines. There are no input parameters. *CONTROL_MPP_IO_NOFULL Purpose: Suppresses the output of the full deck restart files. There are no input parameters. The existence of this keyword suppresses the output of the full deck restart file d3full. *CONTROL_MPP_IO_SWAPBYTES Purpose: Swap bytes on some of the output files. There are no input parameters. The existence of this keyword causes the d3plot file and the “interface component analysis” file to be output with bytes swapped. This is to allow further processing of data on a different machine that has big endian vs. little endian incompatibilities compared to the system on which the analysis is running. *CONTROL_MPP_MATERIAL_MODEL_DRIVER Purpose: Enable this feature in MPP mode. To allow MPP reader to pass the input phase even without any nodes and elements but using only one processor. *CONTROL_MPP_PFILE Purpose: Provide keyword support for the MPP “p=” pfile options All lines of input up to the next keyword card will be copied to a temporary file which is effectively pre-pended to the “p=” file given on the command line (even if no such file is given). This allows all options available via the “p=” file to be specified in the keyword input. The only restriction is that pfile directives in the “directory” section are not available, as those must be processed before the keyword input file is read. See the “LS-DYNA MPP User Guide” in the appendix for details of the available pfile commands and their syntax. *CONTROL_NONLOCAL Purpose: Allocate additional memory for *MAT_NONLOCAL option. Card 1 1 2 3 4 5 6 7 8 Variable MEM Type I Default none VARIABLE MEM DESCRIPTION Percentage increase of memory allocated for *MAT_NONLOCAL option over that required initially. This is for additional storage that may be required due to geometry changes as the calculation proceeds. Generally, a value of 10 should be sufficient. *CONTROL Purpose: Set miscellaneous output parameters. This keyword does not control the information, such as the stress and strain tensors, which is written into the binary databases. For the latter, see the keyword *DATABASE_EXTENT_BINARY. Card 1 1 2 3 4 5 6 7 8 Variable NPOPT NEECHO NREFUP IACCOP OPIFS IPNINT IKEDIT IFLUSH Type Default I 0 I 0 I 0 I 0 F 0. I 0 I I 100 5000 Remaining cards are optional. Optional Card 2 Card 2 1 2 3 4 5 6 7 8 Variable IPRTF IERODE TET10S8 MSGMAX IPCURV GMDT IP1DBLT EOCS Type Default I 0 I 0 I 2 I 50 I 0 F 0. I 0 I 0 Optional Card 3 Card 3 1 2 3 4 5 6 7 8 Variable TOLEV NEWLEG FRFREQ MINFO SOLSIG MSGFLG CDETOL Type Default I 2 I 0 I 1 I 0 I 0 I 0 F 10.0 *CONTROL_OUTPUT Card 4 1 2 3 4 5 6 7 8 Variable PHSCHNG DEMDEN Type Default I 0 I 0 VARIABLE DESCRIPTION NPOPT Print suppression during input phase flag for the “d3hsp” file: EQ.0: no suppression, EQ.1: nodal coordinates, element connectivities, rigid wall definitions, nodal SPCs, initial velocities, initial strains, adaptive constraints, and SPR2/SPR3 constraints are not printed. NEECHO Print suppression during input phase flag for “echo” file: EQ.0: all data printed, EQ.1: nodal printing is suppressed, EQ.2: element printing is suppressed, EQ.3: both node and element printing is suppressed. NREFUP Flag to update reference node coordinates for beam formulations 1, 2, and 11. This option requires that each reference node is unique to the beam: EQ.0: Do not update reference node. EQ.1: Update reference node: This update is required for proper visualization of the beam cross-section orienta- tion in LS-PrePost beyond the initial (𝑡 = 0) plot state. NREFUP does not affect the internal updating of the beam cross-section orientation in LS-DYNA. VARIABLE IACCOP OPIFS IPNINT IKEDIT IFLUSH DESCRIPTION Flag to average or filter nodal accelerations output to file “nodout” and the time history database “d3thdt”: EQ.0: no average (default), EQ.1: averaged between output intervals, EQ.2: accelerations for each time step are stored internally and then filtered over each output interval using a filter from General Motors [Sala, Neal, and Wang, 2004] based on a low-pass Butterworth frequency filter. See also [Neal, Lin, and Wang, 2004]. in *CONTROL_- TIMESTEP must be set to a negative value when IAC- COP = 2 so that the maximum possible number of time steps for an output interval is known and adequate memory can be allocated. See Figure 12.15. DT2MS Output time interval for interface file written per *INTERFACE_- COMPONENT_option. Flag controlling output of initial time step sizes for elements to “d3hsp”: EQ.0: 100 elements with the smallest time step sizes are printed. EQ.1: Time step sizes for all elements are printed. GT.1: IPNINT elements with the smallest time step sizes are printed. Problem status report interval steps to the “d3hsp” file. This flag is ignored if the “glstat” file is written, see *DATABASE_GL- STAT. Number of time steps interval for flushing I/O buffers. The default value is 5000. If the I/O buffers are not emptied and an abnormal termination occurs, the output files can be incomplete. The I/O buffers for restart files are emptied automatically whenever a restart file is written so these files are not affected by this option. IPRTF *CONTROL_OUTPUT DESCRIPTION Default print flag for “rbdout” and “matsum” files. This flag defines the default value for the print flag which can be defined in the part definition section, see *PART. This option is meant to reduce the file sizes by eliminating data which is not of interest. EQ.0: write part data into both matsum and rbdout EQ.1: write data into rbdout file only EQ.2: write data into matsum file only EQ.3: do not write data into rbdout and matsum IERODE Output eroded internal and kinetic energy into the “matsum” file. Also, output to the “matsum” file under the heading of part ID 0 is the kinetic energy from nonstructural mass, lumped mass elements and lumped inertia elements. TET10S8 EQ.0: do not output extra data EQ.1: output the eroded internal and kinetic energy Output ten connectivity nodes for the 10-node solid tetrahedral and the eight connectivity nodes for the 8-node shell into “d3plot” database. The current default is set to 2 since this change in the database may make the data unreadable for many popular post-processors and older versions of LS-PrePost. The default will change to 1 later. EQ.1: write the full node connectivity into the “d3plot” database EQ.2: write only the corner nodes of the elements into the “d3plot” database MSGMAX Maximum number of each error/warning message GT.0: number of messages to screen output, all messages written to d3hsp/messag LE.0: number of messages to screen output and d3hsp/messag EQ.0: default, 50 IPCURV Flag to output digitized curve data to “messag” and d3hsp files. EQ.0: off EQ.1: on VARIABLE GMDT DESCRIPTION Output interval for recorded motions from *INTERFACE_SSI_- AUX IP1DBLT Output information of 1D (bar-type) seatbelt created for 2D (shell- type) seatbelt to sbtout. EQ.0: the analysis results of internally created 1D seatbelts are extracted and processed to yield the 2D belt information. The 2D belt information is stored in sbtout, EQ.1: the analysis results of internally created 1D retractors and slip rings are stored in sbtout. Belt load can be yielded by *DATABASE_CROSS_SECTION. EOCS Elout Coordinate System: controls the coordinate system to be used when writing out shell data to the “elout” file: EQ.0: default EQ.1: local element coordinate system EQ.2: global coordinate system TOLEV NEWLEG FRFREQ Timing Output Levels: controls the # of levels output in the timing summary at termination. The default is 2. New Legends: controls the format of the LEGEND section of various ASCII output files. EQ.0: use the normal format EQ.1: use the optional format with extra fields. Output frequency for failed element report, in cycles. The default is to report the summary every cycle on which an element fails. If > 1, the summary will be reported every FRFREQ cycles whether an element fails that cycle or not, provided some element has failed since the last summary report. Individual element failure is still reported as it occurs. MINFO Output penetration information for mortar contact after each implicit step, not applicable in explicit analysis. See remarks on mortar contact on *CONTACT card. EQ.0: No information EQ.1: Penetrations reported for each contact interface. SOLSIG MSGFLG CDETOL *CONTROL_OUTPUT DESCRIPTION Flag to extrapolate stresses and other history variables for multi- integration point solids from integration points to nodes. These extrapolated nodal values replace the integration point values normally stored in d3plot. When a nonzero SOLSIG is invoked, NINTSLD in *DATABASE_EXTENT_BINARY should be set to 8 as any other value of NINTSLD will result in only one value being reported for each element. Supported solid formulations are: -1, -2, 2, 3, 4, 18, 16, 17, and 23. NOTE: Do not use "Setting - Extrapolate" in LS- PrePost when this field, SOLSIG, is nonzero. EQ.0: No extrapolation. EQ.1: Extrapolate the stress for linear materials only. EQ.2: Extrapolate the stress if plastic strain is zero. EQ.3: Extrapolate the stress always. EQ.4: Extrapolate all history variables. Flag for writing detailed error/warning messages to d3msg. MSGFLG has no affect on length error/warning messages; such messages are written to messag or mes****. NOTE: Most errors/warnings offer only standard length messages. Only a few also offer optional, detailed messages. output of standard EQ.0: Do not write detailed messages to d3msg. EQ.1: Write detailed messages to d3msg at the conclusion of the run. Each detailed message is written only once even in cases where the associated error or warning occurs multiple times. for output of *DEFINE_CURVE discretization Tolerance warnings. After each curve is discretized, the resulting curve is evaluated at each of the original definition points, and the values compared. A warning will be issued for any curve where this comparison results in an error of more than CDETOL/100 × 𝑀, where the curve specific value 𝑀 is computed as the median of the absolute values of the non-zero curve values. VARIABLE PHSCHNG DESCRIPTION Message to messag file when materials 216, 217, and 218 change phase.. EQ.0: (default) no message. EQ.1: The time and element ID are written. DEMDEN Output DEM density data to d3plot database.. EQ.0: (default) no output. EQ.1: output data. *CONTROL_PARALLEL Purpose: Control parallel processing usage by defining the number of processors and invoking the optional consistency of the global vector assembly. This command applies only to shared memory parallel (SMP) LS-DYNA. It does not apply to distributed memory parallel (MPP) LS-DYNA. Card 1 2 3 4 5 6 7 8 Variable NCPU NUMRHS CONST PARA Type Default I 1 Remarks VARIABLE NCPU I 0 1 I 2 2 I 0 3 DESCRIPTION Number of cpus used. (This parameter is disabled in 971 R5 and later versions. Set number of cpus using “ncpu=” on the execution line — see Execution Syntax section of Getting Started — or on the *KEYWORD line of the input.) NUMRHS Number of right-hand sides allocated in memory: EQ.0: same as NCPU, always recommended, EQ.1: allocate only one. CONST Consistency flag. (Including “ncpu=n” on the execution line or on the *KEYWORD line of input overrides CONST. The algebraic sign of n determines the consistency setting.) EQ.1 or n < 0: EQ.2 or n > 0: on (recommended) off, for a faster solution (default). VARIABLE PARA DESCRIPTION Flag for parallel force assembly if CONST=1. (Including “para=” on the execution line overrides PARA.) EQ.0: off EQ.1: on EQ.2: on Remarks: 1. It is recommended to always set NUMRHS = NCPU since great improvements in the parallel performance are obtained since the force assembly is then done in parallel. Setting NUMRHS to one reduces storage by one right hand side vector for each additional processor after the first. If the consistency flag is active, i.e., CONST = 1, NUMRHS defaults to unity. 2. For any given problem with the consistency option off, i.e., CONST = 2, slight differences in results are seen when running the same job multiple times with the same number of processors and also when varying the number of proces- sors. Comparisons of nodal accelerations often show wide discrepancies; how- ever, it is worth noting that the results of accelerometers often show insignificant variations due to the smoothing effect of the accelerometers which are generally attached to nodal rigid bodies. The accuracy issues are not new and are inherent in numerical simulations of automotive crash and impact problems where structural bifurcations under compressive loads are common. This problem can be easily demonstrated by using a perfectly square thin-walled tubular beam of uniform cross section under a compressive load. Typically, every run on one processor that includes a minor input change (i.e., element or hourglass formulation) will produces dramatically different results in terms of the final shape, and, likewise, if the same problem is again run on a different brand of computer. If the same prob- lem is run on multiple processors the results can vary dramatically from run to run WITH NO INPUT CHANGE. The problem here is due to the randomness of numerical round-off which acts as a trigger in a “perfect” beam. Since summations with (CONST=2) occur in a different order from run to run, the round-off is also random. The consistency flag, CONST=1, provides for identical results (or nearly so) whether one, two, or more processors are used while running in the shared memory parallel (SMP) mode. This is done by requiring that all contributions to global vectors be summed in a precise order independently of the number of processors used. When checking for consistent results, nodal displacements or element stresses should be compared. The NODOUT and ELOUT files should be digit to digit identical. However, the GLSTAT, SECFORC, and many of the other ASCII files will not be identical since the quantities in these files are summed in parallel for efficiency reasons and the ordering of summation operations are not enforced. The biggest draw- back of this option is the CPU cost penalty which is at least 15 percent if PA- RA=0 and is much less if PARA=1 and 2 or more processors are used. Unless the PARA flag is on (for non-vector processors), parallel scaling is adversely affected. The consistency flag does not apply to MPP parallel. 3. PARA set to 1 or 2 will cause the force assembly for the consistency option to be performed in parallel for the SMP version, so better scaling will be obtained. However, PARA = 1 will increase memory usage while PARA = 2 will not. This flag does not apply to the MPP version. If PARA = CONST = 0 and NUMRHS = NCPU the force assembly by default is done in parallel, but with- out consistency. The value of the flag may also be given by including “pa- ra=<value>” on the execution line, and the value given in this manner will override the value of PARA in *CONTROL_PARALLEL. *CONTROL Purpose: Set parameters for pore water pressure calculations. This control card is intended for soil analysis. However, other materials containing pore fluid could be treated by the same methods. The pore pressure capabilities invoked by this card are available in SMP and MPP versions of LS-DYNA, but are not available for implicit solutions. Furthermore, pore pressure capabilities are limited to a subset of 3-D solid Lagrangian element formulations, including solid formulations 1, 2, 4, 10, and 15. LS-DYNA uses Terzaghi’s Effective Stress to model materials with pore pressure. The pore fluid and soil skeleton are assumed to occupy the same volume and to carry loads in parallel. Thus, the total stress in an element is the sum of the “effective stress” in the soil skeleton, plus the hydrostatic stress in the pore fluid. LS-DYNA calculates the “effective stress” with standard material models. The pore fluid treatment, then, is independent of material model. The pore pressure is calculated at nodes, and interpolated onto the elements. The pore fluid’s hydrostatic stress is equal to the negative of the element pore pressure. Card 1 1 2 3 4 5 6 7 8 Variable ATYPE (blank) WTABLE PF_RHO GRAV PF_BULK OUTPUT TMF Type Default I 0 F F F F F 0.0 0.0 (none) (none) (none) Card 2 1 2 3 4 5 6 I 0 7 F 1.0 8 Variable TARG FMIN FMAX FTIED CONV CONMAX ETERM THERM Type F F F F F F F F Default 0.0 0.0 0.0 0.0 1.E-4 1.E20 0.0 0.0 *CONTROL_PORE_FLUID Card 3 1 2 3 4 5 6 7 8 Variable ETFLAG Type Default I 0 VARIABLE DESCRIPTION ATYPE Analysis type for pore water pressure calculations: EQ.0: No pore water pressure calculation. EQ.1: Undrained analysis, EQ.2: Drained analysis, EQ.3: Time dependent consolidation (coupled), EQ.4: Consolidate to steady state (uncoupled), EQ.5: Drained in dynamic relaxation, undrained in transient, EQ.6: As 4 but do not check convergence, continue to end time. WTABLE Default z-coordinate of water table (where pore pressure is zero). PF_RHO Default density for pore water. GRAV Gravitational acceleration used to calculate hydrostatic pore water pressure. PF_BULK Default bulk modulus of pore fluid (stress units). OUTPUT Output flag controlling stresses to D3PLOT and D3THDT binary files: EQ.0: total stresses are output EQ.1: effective stresses are output, see notes VARIABLE DESCRIPTION TMF Initial Time Magnification factor on seepage (ATYPE = 3,4 only). TARG FMIN FMAX FTIED CONV GT.0: Factor (can be used with automatic control, see TARG, FMIN, FMAX). LT.0: Load Curve ID giving Time Magnification Factor versus analysis time. Target for maximum change of excess pore pressure at any node, per timestep. If the actual change falls below the target, the time factor on the seepage calculation will be increased . If zero, the constant value of TMF is used. If non-zero, TMF is taken as the initial factor. Minimum time factor on seepage calculation Maximum time factor on seepage calculation Analysis type for pore water pressure calculations: EQ.0.0: Tied contacts act as impermeable membranes, EQ.1.0: Fluid may flow freely through tied contacts. Convergence tolerance for ATYPE = 4. Maximum head change per time step at any node as measured in units of characteristic length, l. 𝑙 = 𝜌𝑔 where, 𝜌 = pore fluid density, PF_ RHO 𝑔 = gravitational acceleration. CONMAX Maximum factor on permeability with ATYPE = -4 ETERM Event time termination (ATYPE = 3) THERM Thermal expansion: Volumetric strain per degree increase for undrained soil. ETFLAG Flag for interpretation of time etc : EQ.0: Time means analysis time, EQ.1: Time means event time. Undrained *CONTROL_PORE_FLUID For analyses of the “undrained” type the pore fluid is trapped within the materi- al. Volume changes result in pore pressure changes. This approximation is used to simulate the effect of rapidly-applied loads on relatively impermeable soil. Drained For analyses of the “drained” type the pore fluid is free to move within the material such that the user-defined pressure-versus-z-coordinate relationship is always maintained. This approximation is used to model high-permeability soils. Time-dependent consolidation For the analysis type “time dependent consolidation,” pressure gradients cause pore fluid to flow through the material according to Darcy’s law: where, v = κ∇(p + z) v = fluid velocity vector κ = permeability p = pressure head z = z-coordinate. Net inflow or outflow at a node leads to a theoretical volume gain or loss. The analysis is coupled, i.e. any difference between actual and theoretical volume leads to pore pressure change, which in turn affects the fluid flow. The result is a prediction of response-versus-time. Steady-state consolidation For the analysis type “steady-state consolidation,” an iterative method is used to calculate the steady-state pore pressure. The analysis is uncoupled, i.e. only the final state is meaningful, not the response-versus-time. Time factoring: Consolidation occurs over time intervals of days, weeks or months. To simulate this process using explicit time integration, a time factor is used. The permeability of the soil is increased by the time factor so that consolidation occurs more quickly. The output times in the D3PLOT and D3THDT files are modified to reflect the time factor. The factored time (“Event Time”) is intended to represent the time taken in the real-life consolidation process and will usually be much larger than the analysis time (the analysis time is the sum of the LS-DYNA timesteps). The time factor may be chosen explicitly (using TMF) but it is recommended to use automatic factoring instead. The automatic scheme adjusts the time factor according to how quickly the pore pressure is changing; usually at the start of consolidation the pore pressure changes quickly and the time factor is low; the time factor increases gradually as the rate of pore pressure change reduces. Automatic time factoring is input by setting TARG (the target pore pressure head change per timestep) and maximum and minimum allowable time factors, for example TARG = 0.001 to 0.01m head, FMIN = 1.0, FMAX = 1.0e6. Optimum settings for these are model-dependent. Loading, other input data from loadcurves, and output time-intervals on *DATABASE cards by default use the analysis time (for example, the x-axis of a loadcurve used for pressure loading is analysis time). When performing consolidation with automatic time-factoring, the relationship between analysis time and event time is unpredictable. Termination based on event time may be input using ETERM. It may also be desired to apply loads as functions of event time rather than analysis time, since the event time is representative of the real-life process. By setting ETFLAG = 2, the time axis of all load curves used for any type of input-versus-time, and output intervals on *DATABASE cards, will be interpreted as event time. This method also allows consolidation to be used as part of a staged construction sequence – when ETFLAG = 2, the stages begin and end at the “real time” stage limits and input curves of pore pressure analysis type vs. time may be used to enforce, for example, consolidation in some stages, and undrained behavior in others. Output: Extra variables for solid elements are automatically written to the d3plot and d3thdt files when the model contains *CONTROL_PORE_FLUID. In LS971 R4 onwards, 5 additional extra variables are written, of which the first is the pore pressure in stress units. In LS971 R3, 15 additional extra variables are written, of which the seventh is pore pressure in stress units. These follow any extra variables requested by the user, e.g. if the user requested 3 extra variables, then in LS971 there will be a total of 8 extra variables of which the fourth is pore pressure. Further optional output to d3plot and d3thdt files is available for nodal pore pressure variables – see *DATABASE_PWP_OUTPUT. For time-dependent and steady-state consolidation, information on the progress of the analysis is written to d3hsp file. Remarks: 1. Tied Contacts. By default, the mesh discontinuity at a tied contact will act as a barrier to fluid flow. If the flag FTIED is set to 1, then pore fluid will be trans- mitted across tied nodes in tied contacts (*CONTACT_TIED_SURFACE_TO_- SURFACE and *CONTACT_TIED_NODES_TO_SURFACE, including_OFFSET and non-_OFFSET types). This algorithm has an effect only when the analysis type of at least one of the contacting parts is 3, 4 or 6. 2. Thermal. Note that this property is for VOLUMETRIC strain increase. Typical thermal expansion coefficients are linear; the volumetric expansion will be three times the linear thermal expansion coefficient. Regular thermal expansion coefficients (e.g. on *MAT or *MAT_ADD_THERMAL_EXPANSION) apply to the soil skeleton and to drained parts. Pore pressure can be generated due to the difference of expansion coefficients of the soil skeleton and pore fluid. 3. Part Associativity. Pore pressure is a nodal variable, but analysis type and other pore pressure related inputs are properties of parts. When a node is shared by elements of different parts, and those parts have different pore pres- sure inputs, the following rules are followed to determine which part’s proper- ties should be applied to the node. a) Dry parts (i.e. parts without a *BOUNDARY_PORE_FLUID card) will never be used (lowest priority). b) If a part is initially dormant (due to staged construction inputs), it has next-lowest priority c) Parts with analysis type = drained have highest priority. d) Next, higher permeability gives higher priority e) If two or more parts have equal-highest priority at a node, the part with lowest ID will win. 4. Related Cards: *BOUNDARY_PORE_FLUID. (This card is essential since without this card, no parts will have pore flu- id.) *BOUNDARY_PWP_OPTION *DATABASE_PWP_OUTPUT *DATABASE_PWP_FLOW *MAT_ADD_PERMEABILITY *CONTROL Purpose: Set parameters for pore air pressure calculations. Card 1 1 2 3 4 5 6 7 8 Variable AIR_RO AIR_P ETERM ANAMSG Type F F F Default (none) (none) endtim I 0 VARIABLE DESCRIPTION PA_RHO Density of atmospheric air, = 1.184 kg/m3 at 25°C PA_PATM Pressure of atmospheric air, = 101.325 kPa at 25°C ETERM ANAMSG Event termination time, default to ENDTIME of *CONTROL_- TERMINATION Flag to turn off the printing of pore air analysis status message, including the analysis time, the node with the highest pressure change. EQ.0: Status messages are printed, the default value. EQ.1: Status messages are not printed *CONTROL_REFINE_ALE Purpose: Refine ALE hexahedral solid elements locally. Each parent element is replaced by 8 child elements with a volume equal to 1/8th the parent volume. If only the 1st card is defined, the refinement occurs during the initialization. The 2nd card defines a criterion CRITRF to automatically refine the elements during the run. If the 3rd card is defined, the refinement can be removed if a criterion CRITRM is reached: the child elements can be replaced by their parents. Card 1 Variable 1 ID 2 3 4 5 6 7 8 TYPE NLVL MMSID IBOX IELOUT Type I Default none I 0 I 1 I 0 I 0 I 0 Remaining cards are optional.† Automatic refinement card. Optional card for activating automatic refinement whereby each element satisfying certain criteria is replaced by a cluster of 8 child elements Card 2 1 2 3 4 5 6 7 8 Variable NTOTRF NCYCRF CRITRF VALRF BEGRF ENDRF LAYRF DELAYRF Type Default I 0 F 0.0 I 0 F F F 0.0 0.0 0.0 I 0 F 0.0 Automatic Refinement Remove Card. Optional card for activating automatic refinement removal whereby, when, for a cluster of 8 child elements, certain criteria are satisfied the clusters is replaced by its parent. Card 3 1 2 3 4 5 6 7 8 Variable MAXRM NCYCRM CRITRM VALRM BEGRM ENDRM MMSRM DELAYRM Type Default I 0 F 0.0 I 0 F F F 0.0 0.0 0.0 I 0 F 0.0 VARIABLE DESCRIPTION ID Set ID. TYPE Set type: EQ.0: ALE Part Set, EQ.1: ALE Part, EQ.2: Lagrangian Part Set coupled to ALE , EQ.3: Lagrangian Part coupled to ALE , EQ.4: Lagrangian Shell Set coupled to ALE , EQ.5: ALE Solid Set. NLVL Number of refinement levels . MMSID Multi-Material Set ID : LT.0: only ALE elements with all the multi-material groups listed in *SET_MULTI-MATERIAL_GROUP_LIST can be refined (or removed otherwise) GT.0: ALE elements with at least one of the multi-material groups can be refined (or removed) IBOX Box ID defining a region in which the ALE elements are refined. IELOUT Flag to handle child data in elout . VARIABLE DESCRIPTION NTOTRF Total number of ALE elements to refine : GT.0: Number of elements to refine EQ.0: NTOTRF = number of solid elements in IBOX LT.0: |NTOTRF| is the id of *CONTROL_REFINE_MPP_DIS- TRIBUTION that computes the number of extra elements required by processors. NCYCRF Number of cycles between each refinement. LT.0: |NCYCRF| is the time interval CRITRF Refinement criterion: EQ.0: static refinement (as if only the 1st card is defined), EQ.1: Pressure (if pressure > VALRF), EQ.2: Relative Volume (if V/Vo < VALRF) , EQ.3: Volume Fraction (if Volume fraction > VALRF), EQ.5: User defined criterion. The fortran routine alerfn_ criteria5 in the file dynrfn_user.f should be used to de- velop the criterion. The file is part of the general package usermat. VALRF Criterion value to reach for the refinement. BEGRF Time to begin the refinement. ENDRF Time to end the refinement. LAYRF Number of element layers to refine around a element reaching the refinement criterion . DELAYRF Period of time after removing the refinement of an element, during which this element will not be refined again. MAXRM Maximum number of child clusters to remove : LT.0: for the whole run, GT.0: every NCYCRM cycles VARIABLE DESCRIPTION NCYCRM Number of cycles between each check for refinement removal: LT.0: |NCYCRM| is the time interval CRITRM Criterion for refinement removal: EQ.0: no refinement removal (as if only the 1st and 2nd card are defined), EQ.1: Pressure (if pressure < VALRM), EQ.2: Relative Volume (if V/Vo > VALRM) , EQ.3: Volume Fraction (if Volume fraction < VALRM), EQ.5: User defined criterion. The fortran routine alermv_ criteria5 in the file dynrfn_user.f should be used to devel- op the criterion. The file is part of the general package usermat. VALRM Criterion value to reach in each child element of a cluster for its removal (child elements replaced by parent element).. BEGRM Time to begin the check for refinement removal: LT.0: |BEGRM| represents a critical percent of NTOTRF below which the check for refinement removal should begin (0.0 < |BEGRM| < 1.0). . ENDRM Time to end the check for refinement removal. MMSRM Multi-Material Set ID for the refinement removal. LT.0: | MMSRM | represents the radius of a sphere centered on a newly refined element, in which the refinement can not be removed. DELAYRM Period of time after refining an element, during which this refinement will not be removed. Remarks: 1. 2. If only the 1st card is defined, only TYPE = 0, 1, 5 can be defined. *CONSTRAINED_LAGRANGE_IN_SOLID needs to be defined for TYPE = 2, 3, 4. If an ALE element has at least one coupling point , this element will be selected to be re- fined (or removed). The number of elements to refine is computed during the initialization. NTOTRF can be zero. Otherwise it can used to add more ele- ments. 3. 4. If NLVL = 1, there is only one level of refinement: the ALE elements in *ELE- MENT_SOLID are the only ones to be replaced by clusters of 8 child elements. If NLVL > 1, there are several levels of refinement: not only the initial ALE elements in *ELEMENT_SOLID are refined but also their child elements. If only the 1st card is defined, a multi-material set id is not used. It can be left to zero. For the 2nd and 3rd cards, MMSID is the ID of *SET_MULTI-MATERIAL_- GROUP_LIST in which the multi-material group ids (as defined in *ALE_MUL- TI-MATERIAL_GROUP) are listed to select the ALE elements to be refined (or removed). If MMSID < 0, only mixed ALE elements containing all the multi- material groups can be refined. Otherwise clusters of 8 elements without a mix of the listed multi-material groups can be removed. 5. NTOTRF defines the total number of ALE elements to be refined. So for example NTOTRF = 100 with NLVL = 1 means that only 100 ALE elements can be replaced by 800 ALE finer elements (or 100 clusters of 8 child elements). For NLVL = 2, these 800 elements can be replaced by 6400 finer elements. 6. 7. 8. If an element is refined, it is possible to refine the neighbor elements as well. LAYRF defines the number of neighbor layers to refine. For example, LAYRF = 2 for an element at the center of a block of 5 × 5 × 5 elements will refine these 125 elements. If MMSRM = 0, MMSID defines the multi-material region where the check for refinement removal should occur. If MMSRM is defined, only ALE child ele- ments fully filled by the multi-material groups listed by the set MMSRM can be removed (if the refinement removal criterion is reached). If BEGRM < 0, the check for refinement removal is activated when the number of 8-element clusters for the refinement is below a limit defined by |BEGRM|*NTOTRF. If |BEGRM| = 0.1, it means that the check for refinement removal starts when 90% of the stock of clusters is used for the refinement. 9. MAXRM < 0 defines a total number of child clusters to remove for the whole run. If positive, MAXRM defines an upper limit for the number of child clus- ters to remove every NCYCRM cycles. 10. If only the 1st card is defined, the code for IELOUT is always activated. Since the refinement occurs during the initialization, every refined element is re- placed by its 8 children in the set defined for *DATABASE_ELOUT. 11. If there are more than 1 line, the code for IELOUT is activated if the flag is equal to 1. Since the refinement occurs during the run, the parent ids in the set de- fined for *DATABASE_ELOUT are duplicated 8NLVL times. The points of inte- gration in the elout file are incremented to differentiate the child contributions to the database. *CONTROL_REFINE_ALE2D Purpose: Refine ALE quadrilateral shell elements locally. Each parent element is replaced by 4 child elements with a volume equal to 1/4th the parent volume. If only the 1st card is defined, the refinement occurs during the initialization. The 2nd card defines a criterion CRITRF to automatically refine the elements during the run. If the 3rd card is defined, the refinement can be removed if a criterion CRITRM is reached: the child elements can be replaced by their parents. Card 1 Variable 1 ID 2 3 4 5 6 7 8 TYPE NLVL MMSID IBOX IELOUT Type I Default none I 0 I 1 I 0 I 0 I 0 Remaining cards are optional.† Automatic refinement card. Optional card for activating automatic refinement whereby each element satisfying certain criteria is replaced by a cluster of 4 child elements Card 2 1 2 3 4 5 6 7 8 Variable NTOTRF NCYCRF CRITRF VALRF BEGRF ENDRF LAYRF Type Default I 0 F 0.0 I 0 F F F 0.0 0.0 0.0 I Automatic Refinement Remove Card. Optional card for activating automatic refinement removal whereby, when, for a cluster of 4 child elements, certain criteria are satisfied the clusters is replaced by its parent. Card 2 1 2 3 4 5 6 7 8 Variable MAXRM NCYCRM CRITRM VALRM BEGRM ENDRM MMSRM Type Default I 0 F 0.0 I 0 F F F 0.0 0.0 0.0 I 0 VARIABLE DESCRIPTION ID Set ID. TYPE Set type: EQ.0: ALE Part Set, EQ.1: ALE Part, EQ.2: Lagrangian Part Set coupled to ALE , EQ.3: Lagrangian Part coupled to ALE , EQ.4: Lagrangian Shell Set coupled to ALE , EQ.5: ALE Shell Set. NLVL Number of refinement levels . MMSID Multi-Material Set ID : LT.0: only ALE elements with all the multi-material groups listed in *SET_MULTI-MATERIAL_GROUP_LIST can be refined (or removed otherwise) GT.0: ALE elements with at least one of the multi-material groups can be refined (or removed) IBOX Box ID defining a region in which the ALE elements are refined. IELOUT Flag to handle child data in elout . VARIABLE DESCRIPTION NTOTRF Total number of ALE elements to refine : GT.0: Number of elements to refine EQ.0: NTOTRF = number of shell elements in IBOX NCYCRF Number of cycles between each refinement. LT.0: |NCYCRF| is the time interval CRITRF Refinement criterion: EQ.0: static refinement (as if only the 1st card is defined), EQ.1: Pressure (if pressure > VALRF), EQ.2: Relative Volume (if V/Vo < VALRF) , EQ.3: Volume Fraction (if Volume fraction > VALRF), EQ.5: User defined criterion: The routine al2rfn_ criteria5 in the file dynrfn_user.f should be used to de- velop the criterion. The file is part of the general pack- age usermat. fortran VALRF Criterion value to reach for the refinement. BEGRF Time to begin the refinement. ENDRF Time to end the refinement. LAYRF Number of element layers to refine around a element reaching the refinement criterion . MAXRM Maximum number of child clusters to remove : LT.0: for the whole run, GT.0: every NCYCRM cycles NCYCRM Number of cycles between each check for refinement removal: LT.0: |NCYCRM| is the time interval VARIABLE DESCRIPTION CRITRM Criterion for refinement removal: EQ.0: no refinement removal (as if only the 1st and 2nd card are defined), EQ.1: Pressure (if pressure < VALRM), EQ.2: Relative Volume (if V/Vo > VALRM) , EQ.3: Volume Fraction (if Volume fraction < VALRM), EQ.5: User defined criterion: The fortran routine al2rmv_ criteria5 in the file dynrfn_user.f should be used to devel- op the criterion. The file is part of the general package usermat. VALRM Criterion value to reach in each child element of a cluster for its removal (child elements of a cluster replaced by parent element). BEGRM Time to begin the check for refinement removal: LT.0: |BEGRM| represents a critical percent of NTOTRF below which the check for refinement removal should begin (0.0 < |BEGRM| < 1.0). . ENDRM Time to end the check for refinement removal. MMSRM Multi-Material Set ID for the refinement removal. Remarks: 1. 2. 3. If only the 1st card is defined, only TYPE = 0,1,5 can be defined. *CONSTRAINED_LAGRANGE_IN_SOLID needs for TYPE = 2,3,4. If an ALE element has at least one coupling point , this element will be selected to be refined (or removed). be defined to If NLVL = 1, there is only one level of refinement: the ALE elements in *ELE- MENT_SHELL are the only ones to be replaced by clusters of 4 child elements. If NLVL > 1, there are several levels of refinement: not only the initial ALE elements in *ELEMENT_SHELL are refined but also their child elements. If NLVL = 2 for example, the initial ALE elements can be replaced by clusters of 16 child elements. 4. If only the 1st card is defined, a multi-material set id is not used. It can be left to zero. For the 2nd and 3rd cards, MMSID is the ID of *SET_MULTI-MATERIAL_- GROUP_LIST in which the multi-material group ids (as defined in *ALE_MUL- TI-MATERIAL_GROUP) are listed to select the ALE elements to be refined (or removed). If MMSID < 0, only mixed ALE elements containing all the multi- material groups can be refined. Otherwise clusters of 4 elements without a mix of the listed multi-material groups can be removed. 5. NTOTRF defines the total number of ALE elements to be refined. So for example NTOTRF = 100 means that only 100 ALE elements will be replaced by 400 ALE finer elements (or 100 clusters of 4 child elements). For NLVL = 2, these 400 elements can be replaced by 1600 finer elements. 6. 7. 8. If an element is refined, it is possible to refine the neighbor elements as well. LAYRF defines the number of neighbor layers to refine. For example, LAYRF = 2 for an element at the center of a block of 5 × 5 elements will refine these 25 elements. If MMSRM = 0, MMSID defines the multi-material region where the check for refinement removal should occur. If MMSRM is defined, only ALE child ele- ments fully filled by the multi-material groups listed by the set MMSRM can be removed (if the refinement removal criterion is reached). If BEGRM < 0, the check for refinement removal is activated when the number of 4-element clusters for the refinement is below a limit defined by |BEGRM|*NTOTRF. If |BEGRM| = 0.1, it means that the check for refinement removal starts when 90% of the stock of clusters is used for the refinement. 9. MAXRM < 0 is the exact opposite of NTOTRF > 0 and it defines a total number of child clusters to remove for the whole run. If positive, MAXRM defines an upper limit for the number of child clusters to remove every NCYCRM cycles 10. If only the 1st card is defined, the code for IELOUT is always activated. Since the refinement occurs during the initialization, every refined element is re- placed by its 4 children in the set defined for *DATABASE_ELOUT. 11. If there are more than 1 line, the code for IELOUT is activated if the flag is equal to 1. Since the refinement occurs during the run, the parent ids in the set de- fined for *DATABASE_ELOUT are duplicated 4NLVL times. The points of inte- gration in the elout file are incremented to differentiate the child contributions to the database. *CONTROL_REFINE_MPP_DISTRIBUTION Purpose: Distribute the elements for the refinement over the MPP processes. This keyword addresses to the following situation: If TYPE = 2, 3, 4 in *CONTROL_REFINE_ALE, the refinement occurs around a structure. The number of elements for this refinement is computed for each process according the initial position of the structure in each MPP subdomain (after the MPP decomposition of the ALE mesh during the phase 3 of the initiali- zation, each process has a subdomain that is a portion of the ALE mesh). If the structure is not in a subdomain, the related process receives no extra element for the refinement. If the structure moves into this subdomain during the computa- tion, the refinement around the structure can not occur. To avoid this problem, the structure can be considered within a box (the structure maxima and minima give the box dimensions and positions). This box moves and expands during the computation to keep the structure inside. An estimation of the maximal dis- placement and expansion will allow the code to evaluate which subdomains the structure will likely cross and how many extra elements a process may need to carry out the refinement. The computation of the number of extra elements per process occurs in 2 steps: • If a file called “refine_mpp_distribution” does not exist in the working directory, it will be created to list the number of elements by process. Each line in this file matches a process rank (starting from 0). After the phase 3 of the MPP decompo- sition, the run terminates as if *CONTROL_MPP_DECOMPOSITION_SHOW was activated. • The model can be run again and the file “refine_mpp_distribution” will be read to allocate the memory for the extra elements and distribute them across the pro- cesses. Card 1 Variable 1 ID Type I 2 DX F 3 DY F 4 DZ F 5 EX F 6 EY F 7 EZ F 8 Default none 0.0 0.0 0.0 1.0 1.0 1.0 VARIABLE DESCRIPTION ID ID = -NTOTRF in *CONTROL_REFINE_ALE VARIABLE DESCRIPTION Dimensionless 𝑥-displacement of the box. . Dimensionless 𝑦-displacement of the box. . Dimensionless 𝑧-displacement of the box. . Dimensionless 𝑥-expansion of the box. . Dimensionless 𝑦-expansion of the box. . Dimensionless 𝑧-expansion of the box. . DX DY DZ EX EY EZ Remarks: 1. Box Displacements. DX, DY and DZ are the maximal displacements of the box center. These displacements are ratio of the box dimensions. If, for exam- ple, the largest length of the structure in the x-direction is 10m and the maximal displacement in this direction is 2m, DX should be equal to 0.2 2. Maximal Box Dilations. EX, EY and EZ represent the maximal dilatations of the box in each direction. These expansions are ratio of the box dimensions. The box expands around its center. If, for example, the maximal thickness of a structure along z is 1cm and the structure deforms 30 times the thickness in z- direction, EZ should be equal to 30 and DZ=15 accounts for the box center mo- tion. The x-y plane is a plane of symmetry for this deformation, DZ can be zero. *CONTROL Purpose: Refine quadrilateral shell elements locally. Each parent element is replaced by 4 child elements with a volume equal to 1/4th the parent volume. If only the 1st card is defined, the refinement occurs during the initialization. The 2nd card defines a criterion CRITRF to automatically refine the elements during the run. If the 3rd card is defined, the refinement can be removed if a criterion CRITRM is reached: the child elements can be replaced by their parents. Card 1 Variable 1 ID 2 3 4 5 6 7 8 TYPE NLVL IBOX IELOUT Type I Default none I 0 I 1 I 0 I 0 Remaining cards are optional.† Automatic refinement card. Optional card for activating automatic refinement whereby each element satisfying certain criteria is replaced by a cluster of 4 child elements Card 2 1 2 3 4 5 6 7 8 Variable NTOTRF NCYCRF CRITRF VALRF BEGRF ENDRF LAYRF Type Default I 0 F 0.0 I 0 F F F 0.0 0.0 0.0 I Automatic Refinement Remove Card. Optional card for activating automatic refinement removal whereby, when, for a cluster of 4 child elements, certain criteria are satisfied the clusters is replaced by its parent. Card 3 1 2 3 4 5 6 7 8 Variable MAXRM NCYCRM CRITRM VALRM BEGRM ENDRM Type Default I 0 F 0.0 I 0 F F F 0.0 0.0 0.0 VARIABLE DESCRIPTION ID Set ID. LT.0: parent elements can be hidden in lsprepost as they are replaced by their children. TYPE Set type:: EQ.0: Part Set, EQ.1: Part, EQ.2: Shell Set. NLVL IBOX Number of refinement levels . Box ID defining a region in which the elements are refined. IELOUT Flag to handle child data in the elout file . NTOTRF Total number of elements to refine : GT.0: Number of elements to refine EQ.0: NTOTRF = number of shell elements in IBOX NCYCRF Number of cycles between each refinement. LT.0: |NCYCRF| is the time interval VARIABLE DESCRIPTION CRITRF Refinement criterion: EQ.0: static refinement (as if only the 1st card is defined), EQ.1: Pressure (if pressure > VALRF), EQ.2: undefined , EQ.3: Von Mises criterion, EQ.4: Criterion similar to ADPOPT = 4 in *CONTROL_ADAP- TIVE (VALRF = ADPTOL), EQ.5: User defined criterion: The routine shlrfn_ criteria5 in the file dynrfn_user.f should be used to devel- op the criterion. The file is part of the general package usermat. fortran VALRF Criterion value to reach for the refinement. BEGRF Time to begin the refinement. ENDRF Time to end the refinement. LAYRF Number of element layers to refine around a element reaching the refinement criterion . MAXRM Maximum number of child clusters to remove : LT.0: for the whole run, GT.0: every NCYCRM cycles NCYCRM Number of cycles between each check for refinement removal: LT.0: |NCYCRM| is the time interval VARIABLE DESCRIPTION CRITRM Criterion for refinement removal: EQ.0: no refinement removal (as if only the 1st and 2nd card are defined), EQ.1: Pressure (if pressure < VALRM), EQ.2: undefined, EQ.3: Von Mises criterion, EQ.4: Criterion similar to ADPOPT = 4 in *CONTROL_ADAP- TIVE (VALRF = ADPTOL), EQ.5: User defined criterion: The fortran routine shlrmv_ criteria5 in the file dynrfn_user.f should be used to de- velop the criterion. The file is part of the general pack- age usermat. VALRM Criterion value to reach in each child elements of a cluster for its removal (child elements replaced by parent element). BEGRM Time to begin the check for refinement removal. LT.0: |BEGRM| represents a critical percent of NTOTRF below which the check for refinement removal should begin (0.0 < |BEGRM| < 1.0). . ENDRM Time to end the check for refinement removal. Remarks: 1. If NLVL = 1, there is only one level of refinement: the elements in *ELEMENT_- SHELL are the only ones to be replaced by clusters of 4 child elements. If NLVL > 1, there are several levels of refinement: not only the initial elements in *ELEMENT_SHELL are refined but also their child elements. If NLVL = 2 for example, the initial elements can be replaced by clusters of 16 child elements. 2. NTOTRF defines the total number of elements to be refined. So for example NTOTRF = 100 with NLVL = 1 means that only 100 elements can be replaced by 400 finer elements (or 100 clusters of 4 child elements). For NLVL = 2, these 400 elements can be replaced by 1600 finer elements. 3. If an element is refined, it is possible to refine the neighbor elements as well. LAYRF defines the number of neighbor layers to refine. For example, LAYRF = 2 for an element at the center of a block of 5 × 5 elements will refine these 25 elements. 4. If BEGRM < 0, the check for refinement removal is activated when the number of 4-element clusters for the refinement is below a limit defined by |BEGRM| × NTOTRF. If |BEGRM| = 0.1, it means that the check for refinement removal starts when 90% of the stock of clusters is used for the refinement. 5. MAXRM < 0 defines a total number of child clusters to remove for the whole run. If positive, MAXRM defines an upper limit for the number of child clus- ters to remove every NCYCRM cycles. 6. 7. If only the 1st card is defined, the code for IELOUT is always activated. Since the refinement occurs during the initialization, every refined element is re- placed by its 4 children in the set defined for *DATABASE_ELOUT. If there are more than 1 line, the code for IELOUT is activated if the flag is equal to 1. Since the refinement occurs during the run, the parent ids in the set de- fined for *DATABASE_ELOUT are duplicated 4NLVL times. The points of inte- gration in the elout file are incremented to differentiate the child contributions to the database. *CONTROL_REFINE_SOLID Purpose: Refine hexahedral solid elements locally. Each parent element is replaced by 8 child elements with a volume equal to 1/8th the parent volume. If only the 1st card is defined, the refinement occurs during the initialization. The 2nd card defines a criterion CRITRF to automatically refine the elements during the run. If the 3rd card is defined, the refinement can be removed if a criterion CRITRM is reached: the child elements can be replaced by their parents. Card 1 Variable 1 ID 2 3 4 5 6 7 8 TYPE NLVL IBOX IELOUT Type I Default none I 0 I 1 I 0 I 0 Remaining cards are optional.† Automatic refinement card. Optional card for activating automatic refinement whereby each element satisfying certain criteria is replaced by a cluster of 8 child elements Card 2 1 2 3 4 5 6 7 8 Variable NTOTRF NCYCRF CRITRF VALRF BEGRF ENDRF LAYRF Type Default I 0 F 0.0 I 0 F F F 0.0 0.0 0.0 I Automatic Refinement Remove Card. Optional card for activating automatic refinement removal whereby, when, for a cluster of 8 child elements, certain criteria are satisfied the clusters is replaced by its parent. Card 2 1 2 3 4 5 6 7 8 Variable MAXRM NCYCRM CRITRM VALRM BEGRM ENDRM Type Default I 0 F 0.0 I 0 F F F 0.0 0.0 0.0 VARIABLE DESCRIPTION ID Set ID. LT.0: parent elements can be hidden in lsprepost as they are replaced by their children. TYPE Set type: EQ.0: Part Set, EQ.1: Part, EQ.2: Solid Set. NLVL IBOX Number of refinement levels. See Remark 1. Box ID defining a region in which the elements are refined. IELOUT Flag to handle child data in elout. See Remarks 6 and 7. NTOTRF Total number of elements to refine. See Remark 2. GT.0: Number of elements to refine EQ.0: NTOTRF = number of solid elements in IBOX NCYCRF Number of cycles between each refinement. LT.0: |NCYCRF| is the time interval VARIABLE DESCRIPTION CRITRF Refinement criterion: EQ.0: static refinement as if only the 1st card is defined, EQ.1: Pressure, if pressure > VALRF, EQ.2: undefined , EQ.3: Von Mises criterion. EQ.5: User defined criterion. The fortran routine sldrfn_ criteria5 in the file dynrfn_user.f should be used to devel- op the criterion. The file is part of the general package usermat. VALRF Criterion value to reach for the refinement. BEGRF Time to begin the refinement. ENDRF Time to end the refinement. LAYRF Number of element layers to refine around an element reaching the refinement criterion. See Remark 3. MAXRM Maximum number of child clusters to remove. See Remark 5. LT.0: for the whole run, GT.0: every NCYCRM cycles NCYCRM Number of cycles between each check for refinement removal: LT.0: |NCYCRM| is the time interval CRITRM Criterion for removal of refinement: EQ.0: no removal of refinement as if only the 1st and 2nd card are defined, EQ.1: Pressure if pressure < VALRM, EQ.2: undefined, EQ.3: Von Mises criterion. EQ.5: User defined criterion. The FORTRAN routine sldrmv_ criteria5 in the file dynrfn_user.f should be used to devel- op the criterion. The file is part of the general package usermat. VARIABLE VALRM DESCRIPTION Criterion value to reach in each child element of a cluster for its removal (replace child elements with parent element). BEGRM Time to begin check for refinement removal: LT.0: |BEGRM| represents a critical percent of NTOTRF below which the check for refinement removal should begin (0.0 < |BEGRM| < 1.0). See Remark 4. ENDRM Time to end the check for refinement removal. Remarks: 1. Number of Refinement Levels. If NLVL=1, there is only one level of refinement: the elements in *ELEMENT_SOLID are the only ones to be replaced by clusters of 8 child elements. If NLVL > 1, there are several levels of refine- ment: not only the initial elements in *ELEMENT_SOLID are refined but also their child elements. If NLVL = 2 for example, the initial elements can be re- placed by clusters of 64 child elements. 2. Maximum Number of Elements to Refine. NTOTRF defines the total number of elements to be refined. So for example NTOTRF=100 with NLVL=1 means that only 100 elements can be replaced by 800 finer elements (or 100 clusters of 8 child elements). For NLVL=2, these 800 elements can be replaced by 6400 finer elements. 3. Number of Layers to Refine. If an element is refined, it is possible to refine the neighbor elements as well. LAYRF defines the number of neighbor layers to refine. For example, LAYRF=2 for an element at the center of a block of 5 × 5 × 5 elements will refine these 125 elements. 4. Onset of Refinement Removal. If BEGRM < 0, the check for refinement removal is activated when the number of 8-element clusters for the refinement is below a limit defined by |BEGRM| × NTOTRF. If |BEGRM| = 0.1, it means that the check for refinement removal starts when 90% of the stock of clusters are used for the refinement. 5. Maximum Refinement Removal. MAXRM < 0 defines a total number of child clusters to remove for the whole run. If positive, MAXRM defines an upper limit for the number of child clusters to remove every NCYCRM cycles. 6. The “elout” Database and Initial Refinement. If only the 1st card is defined, the code for IELOUT is always activated. Since the refinement occurs during the initialization, every refined element is replaced by its 8 children in the set defined for *DATABASE_ELOUT. 7. The “elout” Database and Refinement at Run Time. If there are more than 1 line, the code for IELOUT is activated if the flag is equal to 1. Since the refine- ment occurs during the run, the parent ids in the set defined for *DATABASE_- ELOUT are duplicated 8NLVL times. The points of integration in the elout file are incremented to differentiate the child contributions to the database. *CONTROL_REMESHING_{OPTION} Available options include: <BLANK> EFG Purpose: Provide control over the remeshing of solids which are meshed with the solid tetrahedron element type 13 and mesh-free solid types 41, 42. The element size for three-dimensional adaptivity can be set on the surface mesh of the solid part, and adaptivity can be activated based on the criteria of volume loss, mass increase, or minimum time step size. In addition, so-called interactive adaptivity triggers can be invoked using the EFG option. There are two types of 3-D solid adaptivity affected by *CONTROL_REMESHING: 1. General tetrahedral adaptivity for which the EFG option of *CONTROL_- REMESHING may be invoked. See ADPOPT = 2 in *PART. 2. Axisymmetric adaptivity, sometimes called orbital adaptivity, in which remeshing is done with hexahedral and pentahedral elements. See AD- POPT = 3 in *PART. The EFG option of *CONTROL_REMESHING does not apply for this type of adaptivity. Card 1 1 2 3 4 5 6 7 8 Variable RMIN RMAX VF_LOSS MFRAC DT_MIN ICURV CID SEGANG Type F F F F Default none none 1.0 0.0 F 0. I 4 I 0 F 0.0 Additional card for EFG option. Card 2 1 Variable IVT Type Default I 1 LS-DYNA R10.0 2 IAT I 0 3 4 5 6 7 8 IAAT IER MM I 0 I 0 Second additional card for EFG option. This card is optional. Card 3 1 2 3 4 5 6 7 8 Variable IAT1 IAT2 IAT3 Type F F F Default 1020 1020 1020 VARIABLE DESCRIPTION RMIN RMAX VF_LOSS MFRAC DT_MIN Minimum edge length for the surface mesh surrounding the parts which should be remeshed. Maximum edge length for the surface mesh surrounding the parts which should be remeshed. Volume fraction loss required in a type 13 tetrahedral elements to trigger a remesh. In the type 13 solid elements, the pressures are computed at the nodal points; therefore, it is possible for volume to be conserved but for individual tetrahedrons to experience a significant volume loss or gain. The volume loss can lead to numerical problems. Recommended values for VF_LOSS in the range of 0.10 to 0.30 may be reasonable. Mass ratio gain during mass scaling required for triggering a remesh. For a one percent increase in mass, set MFAC = 0.010. This variable applies to both to general three dimensional tetrahedral remeshing and to three dimensional axisymmetric remeshing. Time step size required for triggering a remesh. This option applies only to general three dimensional tetrahedral remeshing and is checked before mass scaling is applied and the time step size reset. ICURV Define number of element along the radius in the adaptivity. See remark 3. VARIABLE CID DESCRIPTION Coordinate system ID for three dimensional axisymmetric remeshing. The z-axis in the defined coordinate system is the orbital axis, and has to be parallel to the global z-axis in the current axisymmetric remesher. EQ.0: use global coordinate, and the global 𝑧-axis is the orbital axis (default) SEGANG For Axisymmetric 3-D remeshing: Angular element size For General (tet) 3-D remeshing: Critical angle specified in radians to preserve feature lines. (degrees). IVT Internal variable transfer in adaptive EFG. EQ.1: Moving Least square approximation with Kronecker- delta property (recommended in general case). EQ.-1: Moving square Least Kronecker-delta property. approximation without EQ.2: Partition of unity approximation with Kronecker-delta property. EQ.-2: Partition of unity approximation without Kronecker- delta property. EQ.-3: Finite element approximation. IAT Flag for interactive adaptivity. EQ.0: No interactive adaptivity. EQ.1: Interactive adaptivity combined with predefined adaptivity. EQ.2: Purely interactive adaptivity. The time interval between two successive adaptive steps is bounded by ADPFREQ. EQ.3: Purely interactive adaptivity. IAAT Interactive adaptivity adjustable tolerance. EQ.0: The tolerance to trigger interactive adaptivity is not adjusted. EQ.1: The tolerance is adjusted in run-time to avoid over- activation. IER *CONTROL_REMESHING DESCRIPTION Interactive adaptive remeshing with element erosion for metal cutting. EQ.1: The failed elements are eroded and the cutting surface is reconstructed before adaptive remeshing. The current implementation only supports SMP and IAT = 1, 2, 3. MM Interactive adaptive remeshing with monotonic resizing. EQ.1: The adaptive remeshing can not coarsen a mesh. The current implementation only supports IAT = 1, 2, 3 and IER = 0. Shear strain tolerance for interactive adaptivity. If the shear strain in any formulation 42 EFG tetrahedral element exceeds IAT1, remeshing is triggered. (0.1 ~ 0.5 is recommended). 𝐿max/𝐿min tolerance where 𝐿max and 𝐿min are the maximum and minimum edge lengths of any given formulation 42 EFG tetrahedral element. If this ratio in any element exceeds IAT2, remeshing is triggered. (RMAX/RMIN is recommended.) Volume change tolerance. If the normalized change in volume of any formulation 42 tetrahedral element, defined as ∣𝑣1 − 𝑣0∣/∣𝑣0∣ where 𝑣1 is the current element volume and 𝑣0 is the element volume immediately after the most recent remeshing, exceeds IAT3, remeshing is triggered. (0.5 is recommended.) IAT1 IAT2 IAT3 Remarks: 1. The value of RMIN and RMAX should be of the same order. The value of RMAX can be set to 2-5 times greater than RMIN. 2. When interactive adaptivity is invoked (IAT > 0), even if none of the tolerances IAT1, IAT2, and IAT3 for the three respective indicators (shear strain, edge length ratio, normalized volume change) are exceeded, remeshing will still be triggered if any of the three indicators over a single explicit time step changes by more than 50%, that is, if |[value]𝑛 − [value]𝑛−1| |[value]𝑛−1| > 0.5 where [value]𝑛 denotes value of indicator in nth (current) time step and [value]𝑛−1 denotes value of indicator in previous time step . This condition is checked only if [value]𝑛−1 is nonzero. 3. ICURV represents a number of elements and applies only when ADPENE > 0 in *CONTROL_ADAPTIVE. The “desired element size” at each point on slave contact surface is computed based on the tooling radius of curvature , so that ICURV elements would be used to resolve a hypothetical 90 degree arc at the tooling radius of curvature. The value of ICURV is (internally) limited to be >=2 and <=12. The final adapted element size is adjusted as necessary to fall within the size range set forth by RMIN and RMAX. *CONTROL_REQUIRE_REVISION Purpose: To prevent the model from being run in old versions of LS-DYNA. This might be desirable due to known improvements in the program, required capability, etc. Card 1 1 2 3 4 5 6 7 8 Variable RELEASE REVISION Type C I Default none none VARIABLE RELEASE DESCRIPTION The release of code required. This should be a string such as “R6.1.0” or “R7.0” REVISION The minimum revision required. This corresponds to the “SVN Version” field in the d3hsp file. Remarks: 1. Any number of lines can appear, indicating for example that a particular feature was introduced in different release branches at different times. 2. If the RELEASE field is left empty, then any executable whose development split from the main SVN trunk after the given REVISION will be allowed. Example: *CONTROL_REQUIRE_REVISION R6.1 79315 R7.0 78310 78304 This would prevent execution by any R6.1 executable before r79315, any R7.0 before r78310, and all other executables whose development split from the main trunk before r78304. Note that no versions of R6.0, R6.0.0, or R6.1.0 are allowed: R6.1 does NOT imply R6.1.0, no matter what the revision of R6.1.0 – R6.1.0 would have to be explicitly listed. Similarly, R7.0.0 would not be allowed because it is not listed, and it split from the trunk in r76398. Any future R8.X executable would be allowed, since it will have split from the trunk after r78304. *CONTROL_RIGID Purpose: Special control options related to rigid bodies and to linearized flexible bodies, see *PART_MODES. Card 1 1 2 3 4 5 6 7 8 Variable LMF JNTF ORTHMD PARTM SPARSE METALF PLOTEL RBSMS Type Default I 0 I 0 I 0 I 0 I 0 I 0 I 0 I 0 Remaining cards are optional.† Card 2 1 2 3 4 5 6 7 8 Variable NORBIC Type Default I 0 VARIABLE LMF DESCRIPTION Switch the explicit rigid body joint treatment to an implicit impose formulation which uses Lagrange multipliers prescribed kinematic boundary conditions and joint constraints. There is a slight cost overhead due to the assembly of sparse matrix equations which are solved using standard procedures for nonlinear problems in rigid multi-body dynamics. Lagrange multiplier flag: to EQ.0: explicit penalty formulation EQ.1: implicit formulation with Lagrange multipliers VARIABLE DESCRIPTION JNTF Generalized joint stiffness formulation; see Remark 1 below: EQ.0: incremental update EQ.1: total formulation (exact) EQ.2: total formulation intended for implicit analysis ORTHMD Orthogonalize modes with respect to each other: EQ.0: true EQ.1: false, the modes are already orthogonalized PARTM Use global mass matrix to determine part mass distribution. This mass matrix may contain mass from other parts that share nodes. See Remark 2 below. EQ.0: true EQ.1: false SPARSE Use sparse matrix multiply subroutines for the modal stiffness and damping matrices. See Remark 3. EQ.0: false, do full matrix multiplies (frequently faster). EQ.1: true MATELF Metal forming option, which should not be used for crash and other applications involving rigid bodies. Use fast update of rigid body nodes. If this option is active the rotational motion of all rigid bodies should be suppressed. EQ.0: full treatment is used EQ.1: fast update for metal forming applications PLOTEL Automatic generation of *ELEMENT_PLOTEL STRAINED_NODAL_RIGID_BODY. for *CON- EQ.0: no generation EQ.1: one part is generated for all nodal rigid bodies with the PID set to 1000000. EQ.2: one part is generated for each nodal rigid body in the problem with a part ID of 1000000 + PID, where PID is the nodal rigid body ID. RBSMS *CONTROL_RIGID DESCRIPTION Flag to apply consistent treatment of rigid bodies in selective and conventional mass scaling, Remark 4. EQ.0: Off EQ.1: On NORBIC Circumvent rigid body inertia check, see Remark 5. EQ.0: Off EQ.1: On Remarks: 1. JNTF. The default behavior is for the relative angles between the two coordinate systems to be done incrementally. This is an approximation, in contrast to the total formulation where the angular offsets are computed exact- ly. The disadvantage of the latter approach is that a singularity exists when an offset angle equals 180 degrees. In most applications, the stop angles exclude this possibility and JNTF=1 should not cause a problem. JNTF=2 is implement- ed with smooth response and especially intended for implicit analysis. 2. PARTM. If the determination of the normal modes included the mass from both connected bodies and discrete masses, or if there are no connected bodies, then the default is preferred. When the mass of a given part ID is computed, the resulting mass vector includes the mass of all rigid bodies that are merged to the given part ID, but does not included discrete masses. See the keyword: *CONSTRAINED_RIGID_BODIES. A lumped mass matrix is always assumed. 3. SPARSE. Sparse matrix multipliers save a substantial number of operations if the matrix is truly sparse. However, the overhead will slow the multipliers for densely populated matrices. 4. RBSMS. In selective mass scaling, rigid bodies connected to deformable elements can result in significant addition of inertia due missing terms in the SMS mass matrix. This problem has been observed in automotive applications where spotwelds are modeled using constrained nodal rigid bodies. By apply- ing consistent rigid body treatment significant improvement in accuracy and robustness are observed at the expense of increased CPU intensity. This flag also applies to conventional mass scaling as it has been observed that inconsist- encies for various reasons may result in unstable solution schemes even for this case. 5. NORBIC. During initialization, the determinant of the rigid body inertia tensor is checked. If it falls below a tolerance value of 10−30, LS-DYNA issues an error message and the calculation stops. In some rare cases (e.g. with an adverse system of units), such tiny values would still be valid. In this case, NORBIC should be set to 1 to circumvent the implied inertia check. *CONTROL_SHELL Purpose: Provide controls for computing shell response. Card 1 1 2 3 4 5 6 7 8 Variable WRPANG ESORT IRNXX ISTUPD THEORY BWC MITER PROJ Type F Default 20. I 0 I -1 I 0 I 2 I 2 I 1 I 0 Remaining cards are optional.† Card 2 1 2 3 4 5 6 7 8 Variable ROTASCL INTGRD LAMSHT CSTYP6 THSHEL Type F Default 1. Card 3 1 I 0 2 I 0 3 I 1 4 I 0 5 6 7 8 Variable PSTUPD SIDT4TU CNTCO ITSFLG IRQUAD W-MODE STRETCH ICRQ Type Default I 0 I 0 I 0 I 0 I F F I 0 inactive inactive Card 4 1 2 3 4 5 6 7 8 Variable NFAIL1 NFAIL4 PSNFAIL KEEPCS DELFR DRCPSID DRCPRM INTPERR Type I I I Default inactive inactive 0 I 0 I 0 I 0 F 1.0 VARIABLE WRPANG DESCRIPTION Shell element warpage angle in degrees. If a warpage greater than this angle is found, a warning message is printed. Default is 20 degrees. ESORT Sorting of triangular shell elements to automatically switch degenerate quadrilateral shell formulations to more suitable triangular shell formulations. EQ.0: Do not sort (default). EQ.1: Sort (switch to C0 triangular shell formulation 4, or if a quadratic shell, switch to shell formulation 24, or if a shell formulation with thickness stretch, switch to shell formulation 27). EQ.2: Sort (switch to DKT triangular shell formulation 17, or if a quadratic shell, switch to shell formulation 24). The DKT formulation will be unstable if used to model an uncommonly thick, triangular shell. IRNXX Shell normal update option. This option affects the Hughes-Liu, Belytschko-Wong-Chiang, shell formulations (including fully integrated shells -16 and 16). The latter is affected if and only if the warping stiffness option is active, i.e., BWC = 1. the Belytschko-Tsay and EQ.-2: unique nodal fibers which are incrementally updated based on the nodal rotation at the location of the fiber, EQ.-1: recomputed fiber directions each cycle, EQ.0: default set to -1, EQ.1: compute on restarts, EQ.n: compute every n cycles (Hughes-Liu shells only). ISTUPD *CONTROL_SHELL DESCRIPTION Shell thickness change option for deformable shells. The parameter, PSTUPD, on the second optional card allows this option to be applied by part ID. For crash analysis, neglecting the elastic component of the strains, ISTUPD = 4, may improve energy conservation and stability. EQ.0: no thickness change. EQ.1: membrane straining causes thickness change in 3 and 4 node shell elements. This option is very important in sheet metal forming or whenever membrane stretching is important. EQ.2: membrane straining causes thickness change in 8 node thick shell elements, types 1 and 2. This option is not recommended for implicit or explicit solutions which use the fully integrated type 2 elements. Types 3 and 5 thick shells are continuum based and thickness changes are always considered. EQ.3: options 1 and 2 apply. EQ.4: option 1 applies, but the elastic strains are neglected for the thickness update. This option only applies to shells (not thick shells) and the most common elastic-plastic materials for which the elastic response is isotropic. See SIDT4TU for selective application of this option. THEORY list of shell Default shell formulation. For remarks on formulations, refer to *SECTION_SHELL. overriding this default and how THEORY may affect contact behavior, see Remark 2. For a complete EQ.1: Hughes-Liu EQ.2: Belytschko-Tsay (default) EQ.3: BCIZ triangular shell (not recommended) EQ.4: C0 triangular shell EQ.5: Belytschko-Tsay membrane EQ.6: S/R Hughes Liu EQ.7: S/R co-rotational Hughes Liu EQ.8: Belytschko-Leviathan shell EQ.9: fully integrated Belytschko-Tsay membrane VARIABLE DESCRIPTION EQ.10: Belytschko-Wong-Chiang EQ.11: Fast (co-rotational) Hughes-Liu EQ.12: Plane stress (𝑥-𝑦 plane) EQ.13: Plane strain (𝑥-𝑦 plane) EQ.14: Axisymmetric solid (𝑦-axis of symmetry) – area weighted. See Remark 5 EQ.15: Axisymmetric solid (𝑦-axis of symmetry) – volume weighted. See Remark 5 EQ.16: Fully integrated shell element (very fast) EQ.17: Discrete Kirchhoff triangular shell (DKT) EQ.18: Discrete Kirchhoff linear shell either quadrilateral or Triangular with 6DOF per node EQ.20: C0 linear shell element with 6 DOF per node EQ.21: C0 linear shell element with 5 DOF per node with the Pian-Sumihara membrane hybrid quadrilateral mem- brane EQ.25: Belytschko-Tsay shell with thickness stretch EQ.26: Fully integrated shell with thickness stretch EQ.27: C0 triangular shell with thickness stretch BWC Warping stiffness for Belytschko-Tsay shells: EQ.1: Belytschko-Wong-Chiang warping stiffness added. EQ.2: Belytschko-Tsay (default). MITER Plane stress plasticity option (applies to materials 3, 18, 19, and 24): EQ.1: iterative plasticity with 3 secant iterations (default), EQ.2: full iterative plasticity, EQ.3: radial return noniterative plasticity. May lead to false results and has to be used with great care. PROJ Projection method for the warping stiffness in the Belytschko- Tsay shell (the BWC option above) and the Belytschko-Wong- Chiang elements . This parameter applies to explicit calculations since the full projection method is always used if the solution is implicit and this input parameter is VARIABLE DESCRIPTION ignored. EQ.0: drill projection, EQ.1: full projection. ROTASCL Define a scale factor for the rotary shell mass. This option is not for general use. The rotary inertia for shells is automatically scaled to permit a larger time step size. A scale factor other than the default, i.e., unity, is not recommended. INTGRD Default through thickness numerical integration rule for shells and thick shells. If more than 10 integration points are requested, a trapezoidal rule is used unless a user defined rule is specified. EQ.0: Gauss integration: If 1-10 integration points are specified, the default rule is Gauss integration. EQ.1: Lobatto integration: If 3-10 integration points are specified, the default rule is Lobatto. For 2 point integra- tion, the Lobatto rule is very inaccurate, so Gauss inte- gration is used instead. Lobatto integration has an advantage in that the inner and outer integration points are on the shell surfaces. LAMSHT Laminated shell theory flag. Except for those using the Green- Lagrange strain tensor, laminated shell theory is available for all thin shell and thick shell materials. It is activated when LAMSHT = 3, 4, or 5 and by using *PART_COMPOSITE or *IN- TEGRATION_SHELL to define the See Remark 6. integration rule. EQ.0: do not update shear corrections, EQ.1: activate laminated shell theory, EQ.3: activate laminated thin shells, EQ.4: activate laminated shell theory for thick shells, EQ.5: activate laminated shell theory for thin and thick shells. Coordinate system for the type 6 shell element. The default system computes a unique local system at each in plane point. just one system used The uniform local system computes throughout the shell element. This involves fewer calculations and is therefore more efficient. The change of systems has a slight effect on results; therefore, the older, less efficient method is the CSTYP6 VARIABLE DESCRIPTION THSHEL PSTUPD SIDT4TU CNTCO default. EQ.1: variable local coordinate system (default), EQ.2: uniform local system. Thermal shell option (applies only to thermal and coupled structural thermal analyses). See parameter THERM on DATA- BASE_EXTENT_BINARY keyword. EQ.0: No temperature gradient is considered through the shell thickness (default). EQ.1: A temperature gradient is calculated through the shell thickness. |PSTUPD| is the optional shell part set ID specifying which part ID’s have or do not have their thickness updated according to ISTUPD. The shell thickness update as specified by ISTUPD by default applies to all shell elements in the mesh. LT.0: these shell parts are excluded from the shell thickness update EQ.0: all deformable shells have their thickness updated GT.0: these shell parts are included in the shell thickness update Shell part set ID for parts which use the type 4 thickness update where elastic strains are ignored. The shell parts in part set SIDT4TU must also be included in the part set defined by PSTUPD. SIDT4TU has no effect unless ISTUPD is set to 1 or 3. Flag affecting location of contact surfaces for shells when NLOC is nonzero in *SECTION_SHELL or in *PART_COMPOSITE, or when OFFSET is specified using *ELEMENT_SHELL_OFFSET. CNTCO is not supported for the slave side of NODES_TO_SUR- FACE type contacts, neither has it any effect for Mortar contacts. For Mortar contacts NLOC of OFFSET completely determines the location of the contact surfaces, as if CNTCO = 1 would be set. EQ.0: NLOC and OFFSET have no effect on location of shell contact surfaces. EQ.1: Contact reference plane coincides with shell reference surface. EQ.2: Contact reference plane is affected VARIABLE DESCRIPTION by contact thickness. This is typically not physical. For automatic contact types, the shell contact surfaces are always, regardless of CNTCO, offset from a contact reference plane by half a contact thickness. Contact thickness is taken as the shell thickness by default but can be overridden, for example, with input on Card 3 of *CONTACT. The parameter CNTCO affects how the location of the contact reference plane is determined. When CNTCO = 0, the contact reference plane coincides with the plane of the shell nodes. Whereas when CNTCO = 1, the contact reference plane coincides with the shell reference surface as determined by NLOC or by OFFSET. For CNTCO = 2, the contact reference plane is offset from the plane of the nodes by or by – NLOC × contact thickness OFFSET × ( contact thickness shell thickness ) whichever applies. ITSFLG Flag to activate/deactivate initial transverse shear stresses (local shell stress components 𝜎𝑦𝑧 and 𝜎𝑧𝑥) from *INITIAL_STRESS_- SHELL: EQ.0: keep transverse shear stresses EQ.1: set transverse shear stresses to zero IRQUAD In plane integration rule for the 8-node quadratic shell element (shell formulation 23): EQ.2: 2 × 2 Gauss quadrature (default), EQ.3: 3 × 3 Gauss quadrature. Figure 12-86. Illustration of an element in a W-Mode. One pair of opposite corners go up, and the other pair goes down. The angle, 𝛼, is formed by the plane of the flat element and by the vector connecting the center to the corner. See Remark 4. VARIABLE W-MODE STRETCH DESCRIPTION W-Mode amplitude for element deletion, specified in degrees. See Figure 12-86 and Remark 4 for the definition of the angle. Stretch ratio of element diagonals for element deletion. This option is activated if and only if either NFAIL1 or NFAIL4 are nonzero and STRETCH > 0.0. ICRQ Continuous treatment across element edges for some specified result quantities. See Remark 7. NFAIL1 EQ.0: not active EQ.1: thickness and plastic strain Flag to check for highly distorted under-integrated shell elements, print a message, and delete the element or terminate. Generally, this flag is not needed for one point elements that do not use the warping stiffness. A distorted element is one where a negative Jacobian exist within the domain of the shell, not just at integration points. The checks are made away from the CPU requirements for one point elements. If nonzero, NFAIL1 can be changed in a restart. EQ.1: print message and delete element. EQ.2: print message, write d3dump file, and terminate GT.2: print message and delete element. When NFAIL1 elements are deleted then write d3dump file and termi- nate. These NFAIL1 failed elements also include all shell elements that failed for other reasons than distortion. VARIABLE DESCRIPTION NFAIL4 PSNFAIL KEEPCS Before the d3dump file is written, NFAIL1 is doubled, so the run can immediately be continued if desired. Flag to check for highly distorted fully-integrated shell elements, print a message and delete the element or terminate. Generally, this flag is recommended. A distorted element is one where a negative Jacobian exist within the domain of the shell, not just at integration points. The checks are made away from the integration points to enable the bad elements to be deleted before an instability leading to an error termination occurs. If nonzero, NFAIL4 can be changed in a restart. EQ.1: print message and delete element. EQ.2: print message, write d3dump file, and terminate GT.2: print message and delete element. When NFAIL4 elements are deleted then write d3dump file and termi- nate. These NFAIL4 failed elements also include all shell elements that failed for other reasons than distortion. Before the d3dump file is written, NFAIL4 is doubled, so the run can immediately be continued if desired. Optional shell part set ID specifying which part ID’s are checked by the NFAIL1, NFAIL4, and W-MODE options. If zero, all shell part ID’s are included. Flag to keep the contact segments of failed shell elements in the calculation. The contact segments of the failed shells remain active until a node shared by the segments has no active shells attached. Only then are the segments deleted. EQ.0: Inactive EQ.1: Active DELFR Flag to delete shell elements whose neighboring shell elements have failed; consequently, the shell is detached from the structure and moving freely in space. This condition is checked if NFAIL1 or NFAIL4 are nonzero. EQ.0: Inactive EQ.1: Isolated elements are deleted. EQ.2: Isolated quadrilateral elements and triangular elements connected by only one node are deleted. VARIABLE DESCRIPTION EQ.3: Elements that are either isolated or connected by only one node are deleted. DRCPSID Part set ID for drilling rotation constraint method . DRCPRM Drilling rotation constraint parameter (default = 1.0). INTPERR Flag for behavior in case of unwanted interpolation/extrapolation of initial stresses from *INITIAL_STRESS_SHELL. EQ.0: Only warning is written, calculation continues (default). EQ.1: Error exit, calculation stops. Remarks: 1. Drill versus Full Projections for Warping Stiffness. The drill projection is used in the addition of warping stiffness to the Belytschko-Tsay and the Be- lytschko-Wong-Chiang shell elements. This projection generally works well and is very efficient, but to quote Belytschko and Leviathan: "The shortcoming of the drill projection is that even elements that are in- variant to rigid body rotation will strain under rigid body rotation if the drill projection is applied. On one hand, the excessive flexibility rendered by the 1-point quadrature shell element is corrected by the drill projection, but on the other hand the element becomes too stiff due to loss of the rigid body rotation invariance under the same drill projection". They later went on to add in the conclusions: "The projection of only the drill rotations is very efficient and hardly in- creases the computation time, so it is recommended for most cases. How- ever, it should be noted that the drill projection can result in a loss of invariance to rigid body motion when the elements are highly warped. For moderately warped configurations the drill projection appears quite accu- rate". In crashworthiness and impact analysis, elements that have little or no warpage in the reference configuration can become highly warped in the deformed con- figuration and may affect rigid body rotations if the drill projection is used, i.e., DO NOT USE THE DRILL PROJECTION. Of course it is difficult to define what is meant by "moderately warped". The full projection circumvents these problems but at a significant cost. The cost increase of the drill projection ver- sus no projection as reported by Belytschko and Leviathan is 12 percent and by timings in LS-DYNA, 7 percent, but for the full projection they report a 110 percent increase and in LS-DYNA an increase closer to 50 percent is observed. In Version 940 of LS-DYNA the drill projection was used exclusively, but in one problem the lack of invariance was observed; consequently, the drill projection was replaced in the Belytschko-Leviathan shell with the full projection and the full projection is now optional for the warping stiffness in the Belytschko-Tsay and Belytschko-Wong-Chiang elements. Starting with version 950 the Be- lytschko-Leviathan shell, which now uses the full projection, is somewhat slow- er than in previous versions. In general, in light of these problems, the drill projection cannot be recommended. For implicit calculations, the full projection method is used in the development of the stiffness matrix. 2. THEORY, ELFORM, and Contact with Tapered Shells. All shell parts need not share the same element formulation. A nonzero value of ELFORM, given either in *SECTION_SHELL or *PART_COMPOSITE, overrides the element formulation specified by THEORY in *CONTROL_SHELL. When using MPP, THEORY = 1 in *CONTROL_SHELL has special meaning when dealing with non-uniform-thickness shells, that is, it serves to set the nodal contact thickness equal to the average of the nodal thicknesses from the shells sharing that node. Thus when a contact surface is comprised of non- uniform-thickness shells, THEORY = 1 is recommended and the user still has the option of setting the actual shell theory using ELFORM in *SECTION_ SHELL. 3. Drilling Rotation Constraint Method. The drilling rotation constraint method which is used by default in implicit calculations can be used in explicit calculations as well by defining an appropriate part set DRCPSID. This might be helpful in situations where single constraints (e.g. spotwelds) are connected to flat shell element topologies. The additional drill force can by scaled with DRCPRM (default value is 1.0), where a moderate value should be chosen to avoid excessive stiff- ening of the structure. A speed penalty of max. 15 % may be observed with this option. 4. W-Mode Failure Criterion. The w-mode failure criteria depends on the magnitude of the w-mode, 𝑤, compared to the approximate side-length ℓ. The magnitude, 𝑤, is defined as 𝑤 = [(𝐱1 − 𝐱2) + (𝐱3 − 𝐱4)] ⋅ 𝐧 where 𝐱𝑖 is the position vector for node 𝑖, and 𝐧 is the element normal vector evaluated at the centroid. The element normal is the unit vector obtained from the cross product of the diagonal vectors 𝐚 and 𝐛 as, 𝐚 = 𝐱3 − 𝐱1 𝐛 = 𝐱4 − 𝐱2 𝐧 = 𝐚 × 𝐛 ‖𝐚 × 𝐛‖ . The failure criteria depends on the ratio of 𝑤 to ℓ, where ℓ is defined as, ℓ = ⎤ ⎡ ⎥ ⎢ √2 √ ⎥ ⎢ ⎥ ⎢ ⎣ ⎦ ⏟⏟⏟⏟⏟⏟⏟ ~diagonal length ‖𝐚 × 𝐛‖ ⏟⏟⏟⏟⏟ ~√area such that the element is deleted when |𝑤| ≥ tan(WMODE). The angle 𝛼 in the figure may be identified as, α = arctan ( |𝑤| ). 5. 2D Axisymmetric Solid Elements. The 2D axisymmetric solid elements come in two types: area weighted (type 14) and volume weighted (type 15). a) High explosive applications work best with the area weighted approach and structural applications work best with the volume weighted ap- proach. The volume weighted approach can lead to problems along the axis of symmetry under very large deformations. Often the symmetry condition is not obeyed, and the elements will kink along the axis. b) The volume weighted approach must be used if 2D shell elements are used in the mesh. Type 14 and 15 elements cannot be mixed in the same calculation. 6. Lamination Theory. Lamination theory should be activated when the assumption that shear strain through the shell is uniform and constant becomes violated. Unless this correction is applied, the stiffness of the shell can be gross- ly incorrect if there are drastic differences in the elastic constants from ply to ply, especially for sandwich type shells. Generally, without this correction the results are too stiff. For the discrete Kirchhoff shell elements, which do not consider transverse shear, this option is ignored. For thin shells of material *MAT_ENHANCED_COMPOSITE_ types, DAMAGE, and *MAT_GENERAL_VISCOELASTIC, laminated shell theory may also be done by stiffness correction by setting LAMSHT=1. *MAT_COMPOSITE_DAMAGE, 7. Continuous Result Quantities. A nodal averaging technique is used to achieve continuity for some quantities across element edges. Applying this approach to the thickness field and plastic strains (ICRQ=1) can reduce alternat- ing weak localizations sometimes observed in metal forming applications when shell elements get stretch-bended over small radii. This option currently works with shell element types 2, 4, and 16. A maximum number of 9 through thick- ness integration points is allowed for this method. A speed penalty of max. 15 % may be observed with this option. Purpose: Provide controls for solid element response. *CONTROL Card 1 1 2 3 4 5 6 7 8 Variable ESORT FMATRX NIPTETS SWLOCL PSFAIL T10JTOL ICOH TET13K Type Default I 0 I 0 I 4 I 1 I 0 F 0. I 0 I 0 This card is optional. Card 2 1 2 3 4 5 6 7 8 9 10 Variable PM1 PM2 PM3 PM4 PM5 PM6 PM7 PM8 PM9 PM10 Type I I I I I I I I I I Default none none none none none none none none none none VARIABLE ESORT DESCRIPTION Automatic sorting of tetrahedral and pentahedral elements to avoid use of degenerate formulations for these shapes. See *SEC- TION_SOLID. EQ.0: no sorting (default) EQ.1: sort tetrahedron to type 10; pentahedron to type 15; cohesive pentahedron types 19 and 20 to types 21 and 22, respectively. EQ.2: sort to tetrahedron integrated pentahedron to type 115; fully integrated pentahedron to type 15; cohesive pentahedron types 19 and 20 to types 21 and 22, respectively. type 10; 1-point EQ.3: same as EQ.1 but also print switched elements in messag file EQ.4: same as EQ.2 but also print switched elements in messag file FMATRX NIPTETS SWLOCL PSFAIL T10JTOL *CONTROL_SOLID DESCRIPTION Default method used in the calculation of the deformation gradient matrix. EQ.1: Update incrementally in time. This is the default for explicit. EQ.2: Directly compute F: This is the default for implicit and implicit/explicit switching. Number of integration points used in the quadratic tetrahedron elements. Either 4 or 5 can be specified. This option applies to the types 4, 16, and 17 tetrahedron elements. Output option for stresses in solid elements used as spot welds with material and d3plot/d3part/etc. *MAT_SPOTWELD. Affects elout EQ.1: Stresses in global coordinate system (default), EQ.2: Stresses in element coordinate system. A nonzero PSFAIL has the same effect as setting ERODE = 1 in *CONTROL_TIMESTEP except that solid element erosion due to negative volume is limited to only the solid elements in part set PSFAIL. In other words, when PSFAIL is nonzero, the time-step-based criterion for erosion (TSMIN) applies to all solid elements (except formulations 11 and 12) while the negative volume criterion for erosion applies only to solids in part set PSFAIL. Tolerance for jacobian in 4-point 10-noded quadratic tetrahedra (type 16). If the quotient between the minimum and maximum jacobian value falls below this tolerance, a warning message is issued in the messag file. This is useful for tracking badly shaped elements in implicit analysis that deteriorates convergence, a value of 1.0 indicates a perfectly shaped element. VARIABLE ICOH TET13K PM1 – PM10 DESCRIPTION Global flag for cohesive element options, interpreted digit-wise as follows: ICOH = [𝐿𝐾] = 𝐾 + 10 × 𝐿 K.EQ.1: Solid elements having ELFORM = 19-22 will be eroded when neighboring shell or solid elements fail. Only works for nodewise connected parts, not tied contacts. K.EQ.0: No cohesive element deletion due to neighbor failure. L.EQ.0: Default critical time step estimate. L.EQ.1: Most conservative estimate. (smallest) critical time step L.EQ.2: Intermediate critical time step estimate. Set to 1 to invoke a consistent tangent stiffness matrix for the pressure averaged tetrahedron (type 13). This feature is available only for the implicit integrator and it is not supported in the MPP/MPI version. This element type averages the volumetric strain over adjacent elements to alleviate volumetric locking, therefore, the corresponding material tangent stiffness should be treated accordingly. In contrast to a hexahedral mesh where a node usually connects to fewer than 8 elements, tetrahedral meshes offer no such regularity. Consequently, for nonlinear implicit analysis matrix assembly is computationally expensive and this option is recommended only for linear or eigenvalue analysis to exploit the stiffness characteristics of the type 13 tetrahedron. Components of a permutation vector for nodes that define the 10- node tetrahedron. The nodal numbering of 10-node tetrahedron elements is somewhat arbitrary. The permutation vector allows other numbering schemes to be used. Unless defined, this permutation vector is not used. PM1 – PM10 are unique numbers between 1 to 10 inclusive that reorders the input node ID’s for a 10-node tetrahedron into the order used by LS-DYNA. *CONTROL_SOLUTION Purpose: To specify the analysis solution procedure if thermal only or coupled thermal analysis is performed. Other solutions parameters including the vector length and NaN (not a number) checking can be set. Card 1 1 2 3 4 5 6 7 8 Variable SOLN NLQ ISNAN LCINT LCACC Type Default I 0 I 0 I 0 I 100 I 0 VARIABLE DESCRIPTION SOLN Analysis solution procedure: NLQ ISNAN LCINT EQ.0: Structural analysis only, EQ.1: Thermal analysis only, EQ.2: Coupled structural thermal analysis. Define the vector length used in solution. This value must not exceed the vector length of the system which varies based on the machine manufacturer. The default vector length is printed at termination in the messag file. Flag to check for a NaN in the force and moment arrays after the assembly of these arrays is completed. This option can be useful for debugging purposes. A cost overhead of approximately 2% is incurred when this option is active. EQ.0: No checking, EQ.1: Checking is active. Number of equally spaced points used in curve (*DEFINE_- CURVE) rediscretization. Curve rediscretization applies only to curves used in material models. Curves defining loads, motion, etc. are not rediscretized. VARIABLE LCACC DESCRIPTION Flag to truncate curves to 6 significant figures for single precision and 13 significant figures for double precision. The truncation is done after applying the offset and scale factors specified in *DE- FINE_CURVE. Truncation is intended to prevent curve values from deviating from the input value, e.g., 0.7 being stored as 0.69999999. This small deviation was seen to have an adverse effect in a particular analysis using *MAT_083. In general, curve truncation is not necessary and is unlikely to have any effect on results. EQ.0: No truncation. NE.0: Truncate. *CONTROL_SPH Purpose: Provide controls relating to SPH (Smooth Particle Hydrodynamics). Card 1 1 2 Variable NCBS BOXID Type Default I 1 I 0 3 DT F 4 5 6 7 8 IDIM MEMORY FORM START MAXV I I 1020 none 150 I 0 F F 0.0 1015 Optional Card. Card 2 1 2 Variable CONT DERIV Type Default I 0 I 0 3 INI I 0 4 5 6 7 8 ISHOW IEROD ICONT IAVIS ISYMP I 0 I 0 I 0 I 0 I 100 VARIABLE DESCRIPTION NCBS Number of time steps between particle sorting. BOXID DT IDIM SPH approximations are computed inside a specified BOX. When a particle has gone outside the BOX, it is deactivated. This will save computational time by eliminating particles that no longer interact with the structure. Death time. Determines when the SPH calculations are stopped. Space dimension for SPH particles: EQ.3: for 3D problems EQ.2: for 2D plane strain problems EQ.-2: for 2D axisymmetric problems MEMORY Defines the initial number of neighbors per particle . VARIABLE DESCRIPTION FORM Particle approximation theory (Remark 2): EQ.0: default formulation EQ.1: renormalization approximation EQ.2: symmetric formulation EQ.3: symmetric renormalized approximation EQ.4: tensor formulation EQ.5: fluid particle approximation EQ.6: fluid particle with renormalization approximation EQ.7: total Lagrangian formulation EQ.8: total Lagrangian formulation with renormalization EQ.15: enhanced fluid formulation EQ.16: enhanced fluid formulation with renormalization Start time for particle approximation. Particle approximations will be computed when time of the analysis has reached the value defined in START. Maximum value for velocity for the SPH particles. Particles with a velocity greater than MAXV are deactivated. A negative MAXV will turn off the velocity checking. Defines the computation of the particle approximation between different SPH parts: EQ.0: Particle approximation is defined (default) EQ.1: Particle approximation is not computed. Different SPH materials will not interact with each other and penetra- tion is allowed unless *DEFINE_SPH_TO_SPH_COU- PLING is defined. Combined with *SECTION_SPH_IN- TERACTION, a partial interaction between SPH parts through normal interpolation method and partially in- teract through the contact option can be realized. See *SECTION_SPH_INTERACTION. START MAXV CONT DERIV Time integration type for the smoothing length: EQ.0: 𝑑 EQ.1: 𝑑 𝑑𝑡 [ℎ(𝑡)] = 1 𝑑𝑡 [ℎ(𝑡)] = 1 𝑑 ℎ(𝑡)∇ ⋅ 𝐯, (default), 𝑑 ℎ(𝑡)(∇ ⋅ 𝐯)1/3 VARIABLE DESCRIPTION INI Computation of the smoothing length during the initialization: EQ.0: Bucket sort based algorithm (default, very fast). EQ.1: Global computation on all the particles of the model. EQ.2: Based on the mass of the SPH particle. ISHOW Display option for deactivated SPH particles: EQ.0: No distinction in active SPH particles and deactivated SPH particles when viewing in LS-PrePost. EQ.1: Deactivated SPH particles are displayed only as points and active SPH particles are displayed as spheres when Setting → SPH → Style is set to “smooth” in LS-PrePost. IEROD Deactivation control for SPH particles: EQ.0: Particles remain active. EQ.1: SPH particles are partially deactivated and stress states are set to 0 when erosion criteria are satisfied. See Re- mark 3. EQ.2: SPH particles are totally deactivated and stress states are set to 0 when erosion criteria are satisfied. See Remark 3. ICONT Controls contact behavior for deactivated SPH particles: EQ.0: Any contact defined for SPH remains active for deactivated particles. EQ.1: Contact is inactive for deactivated particles. IAVIS Defines artificial viscosity formulation for SPH elements (Remark 4): ISYMP EQ.0: Monaghan type artificial viscosity formulation is used. EQ.1: Standard type artificial viscosity formulation from solid element is used (this option is not supported in SPH 2D and 2D axisymmetric elements). Defines the percentage of original SPH particles used for memory allocation of SPH symmetric planes ghost nodes generation process (default is 100%). Recommended for large SPH particles models (value range 10~20) to control the memory allocation for SPH ghost particles with *BOUNDARY_SPH_SYMMETRY_- PLANE keyword. *CONTROL 1. Memory. MEMORY is used to determine the initial memory allocation for the SPH arrays. Its value can be positive or negative. If MEMORY is positive, memory allocation is dynamic such that the number of neighboring particles is initially equal to MEMORY but that number is subsequently allowed to exceed MEMORY as the solution progresses. If MEMORY is negative, memory alloca- tion is static and |MEMORY| is the maximum allowed number of neighboring particles for each particle throughout the entire solution. Using this static memory option can avoid memory allocation problems. 2. Form. Some guidelines for selecting form variable: for most solid structure applications, form = 1 is recommended for more accurate results around the boundary area; for fluid or fluid-like material applications, form = 15, 16 with fluid formulation are recommended (form=16 usually has better accuracy but requires more CPU time); form = 2, 3 are not recommended for any case; all SPH formulations with Eulerian kernel (form = 0 to 6, 15 and 16) can be used for large or extreme large deformation applications but will have tensile insta- bility issue; all SPH formulations with Lagrangian kernel (form = 7,8) can be used to avoid tensile instability issue but they can not endure very large defor- mation, user has to be careful to pick up the right one based on the applications. Only formulations 0, 1, 15 and 16 are implemented for 2D axisymmetric prob- lems (dim=-2). Also note that forms 15 and 16 include a smoothing of the pres- sure field, and are therefore not recommended for materials with failure or problems with important strain localization. 3. Erosion. The erosion criteria, which triggers particle deactivation when IEROD=1 or 2, may come from either the material model with *MAT_ADD_- EROSION or from the ERODE parameter in *CONTROL_TIMESTEP. For IER- OD=1, SPH particles are partially deactivated (i.e. the stress states of the deactivated SPH particles will be set to 0, but those particles still remain in the domain integration for more stable results); For IEROD=2, SPH particles are totally deactivated: stress states will be set to 0 and the deactivated particles no more remain in the domain integration. Deactivated particles can be distin- guished from active particles by setting ISHOW=1. To disable contact for deac- tivated particles, set ICONT=1. 4. Artificial Viscosity. The artificial viscosity for standard solid elements, which is active when AVIS=1, is given by: 2 − 𝑄2𝑎𝜀̇𝑘𝑘) 𝑞 = 𝜌𝑙(𝑄1𝑙𝜀̇𝑘𝑘 𝑞 = 0 𝜀̇𝑘𝑘 < 0 𝜀̇𝑘𝑘 ≥ 0 where 𝑄1 and 𝑄2 are dimensionless input constants which default to 1.5 and .06, respectively, and 𝑙 is a characteristic length given as the square root of the area in two dimensions and as the cube root of the volume in three, 𝑎 is the local sound speed. This formulation, which is consistent with solid artificial viscosi- ty, has better energy balance for SPH elements. For general applications, Mon- aghan type artificial viscosity is recommended since this type of artificial viscosity is specifically designed for SPH particles. The Monaghan type artificial viscosity, which is active when AVIS = 0, is de- fined as follows: 𝑞 = ⎧−𝑄2𝑐𝑖𝑗𝜙𝑖𝑗 + 𝑄1𝜙𝑖𝑗 {{ 𝜌𝑖𝑗 ⎨ {{ ⎩ 𝑣𝑖𝑗𝑥𝑖𝑗 < 0 𝑣𝑖𝑗𝑥𝑖𝑗 ≥ 0 Where, 𝜙𝑖𝑗 = ℎ𝑖𝑗𝑣𝑖𝑗𝑥𝑖𝑗 ∣𝑥𝑖𝑗∣ + 𝜑2 𝑐 ̅𝑖𝑗 = 0.5(𝑐𝑖 + 𝑐𝑗) 𝜌̅𝑖𝑗 = 0.5(𝜌𝑖 + 𝜌𝑗) ℎ𝑖𝑗 = 0.5(ℎ𝑖 + ℎ𝑗) 𝜑 = 0.1ℎ𝑖𝑗 𝑄1, 𝑄2 are input constants. When using Monaghan type artificial viscosity, it is recommended that the user set both Q1 and Q2 to 1.0 on either the *CON- TROL_BULK_VISCOSITY or *HOURGLASS keywords; see for example G. R. Liu. *CONTROL Purpose: Provides factors for scaling the failure force resultants of beam spot welds as a function of their parametric location on the contact segment and the size of the segment. Also, an option is provided to replace beam welds with solid hexahedron element clusters. Card 1 1 2 3 4 5 6 7 8 Variable LCT LCS T_ORT PRTFLG T_ORS RPBHX BMSID ID_OFF Type Default I 0 I 0 I 0 I 0 I 0 I 0 I 0 I 0 VARIABLE DESCRIPTION LCT LCS T_ORT PRTFLG Load curve ID for scaling the response in tension based on the shell element size. Load curve ID for scaling the response in shear based on the shell element size. Table ID for scaling the tension response (and shear response if T_ORS = 0) based on the location of the beam node relative to the centroid of the shell. Set this flag to 1 to print for each spot weld attachment: the beam, node, and shell ID’s, the parametric coordinates that define the constraint location, the angle used in the table lookup, and the three scale factors obtained from the load curves and table lookup. See Figure 12-87. Figure 12-87. Definition of parameters for table definition. VARIABLE DESCRIPTION Optional table ID for scaling the shear response based on the location of the beam node relative to the centroid of the shell. Replace each spot weld beam element with a cluster of RPBHX solid elements. The net cross-section of the cluster of elements is dimensioned to have the same area as the replaced beam. RPBHX may be set to 1, 4, or 8. When RPBHX is set to 4 or 8, a table is generated to output the force and moment resultants into the SWFORC file, if this file is active. This table is described by the keyword: *DEFINE_HEX_SPOTWELD_ASSEMBLY. The ID’s of the beam elements are used as the cluster spot weld ID’s so the ID’s in the SWFORC file are unchanged. The beam elements are automatically deleted from the calculation, and the section and material data is automatically changed to be used with solid elements. See Figure 11-24. Optional beam set ID defining the beam element ID’s that are to be converted to hex assemblies. If zero, all spot weld beam elements are converted to hex assemblies. This optional ID offset applies if and only if BMSID is nonzero. Beams, which share part ID’s with beams that are converted to hex assemblies, will be assigned new part ID’s by adding to the original part ID the value of ID_OFF. If ID_OFF, is zero the new part ID for such beams will be assigned to be larger than the largest part ID in the model. T_ORS RPBHX BMSID ID_OFF Remarks: The load curves and table provide a means of scaling the response of the beam spot welds to reduce any mesh dependencies for failure model 6 in *MAT_SPOTWELD. Figure 12-88 shows such dependencies that can lead to premature spot weld failure. Separate scale factors are calculated for each of the beam’s nodes. The scale factors sT, sS, sOT , and sOS are calculated using the load curves LCT, LCS, table T_ORT, and table T_ORS, respectively, and are introduced in the failure criteria, ⎢⎡𝑠𝑇𝑠𝑂𝑇𝜎𝑟𝑟 ⎥⎤ 𝐹 (𝜀̇𝑒𝑓𝑓 )⎦ 𝜎𝑟𝑟 ⎣ + ⎢⎡ 𝑠𝑆𝑠𝑂𝑆𝜏 ⎥⎤ 𝜏𝐹(𝜀̇𝑒𝑓𝑓 )⎦ ⎣ − 1 = 0 If a curve or table is given an ID of 0, its scale factor is set to 1.0. The load curves LCT and LCS are functions of the characteristic size of the shell element used in the time step calculation at the start of the calculation. The orientation table is a function of the spot weld’s isoparametric coordinate location on the shell element. A vector V=(s,t) is defined from the centroid of the shell to the contact point of the beam’s node. The arguments for the orientation table are the angle: Θ = tan−1 [ min(|𝑠|, |𝑡|) max(|𝑠|, |𝑡|) ], and the normalized distance 𝑑 ̅= 𝑑 𝐷⁄ = max(|𝑠|, |𝑡|). See Figure 12-87 The table is periodic over a range of 0 (V aligned with either the s or t axis) to 45 degrees (V is along the diagonal of the element). The table is specified by the angle of V in degrees, ranging from 0 to 45, and the individual curves give the scale factor as a function of the normalized distance of the beam node, 𝑑̅̅̅̅̅̅ , for a constant angle. 1.20 1.00 0.80 0.60 0.40 0.20 0.00 1.20 1.00 0.80 0.60 0.40 0.20 0.00 _ . _ . CROSS TENSION EDGE DIRECTION . 1.20 1.00 0.80 0.60 0.40 0.20 0.00 Both side One side dynamic static 10 12 Center Point1 Point2 Point3 Point4 Edge MESH SIZE (mm) SHEAR dynamic static SPOT BEAM LOCATION CORNER DIRECTION Both side One side . 1.20 1.00 0.80 0.60 0.40 0.20 0.00 10 12 MESH SIZE (mm) Center Point1 Point2 Point3 Point4 Corner SPOT BEAM LOCATION Figure 12-88 The failure force resultants can depend both on mesh size and the location of weld relative to the center of the contact segment Purpose: Define the start time of analysis. *CONTROL Card 1 1 2 3 4 5 6 7 8 Variable BEGTIM Type F VARIABLE BEGTIM DESCRIPTION Start time of analysis (default = 0.0). Load curves are not shifted to compensate for the time offset. Therefore, this keyword will change the results of any calculation involving time-dependent load curves. *CONTROL_STAGED_CONSTRUCTION This control card is used to help break down analyses of construction processes into stages. Card 1 1 2 3 4 5 6 7 8 Variable TSTART STGS STGE ACCEL FACT STREF DORDEL NOPDEL Type Default F 0 I 0 I 0 F F 0.0 1.e-6 I 0 I 0 I 0 VARIABLE DESCRIPTION TSTART Time at start of analysis (normally leave blank) STGS STGE Construction stage at start of analysis Construction stage at end of analysis ACCEL Default acceleration for gravity loading FACT Default stiffness and gravity factor for parts before they are added STREF Reference stage for displacements in d3plot file DORDEL Dormant part treatment in d3plot file, see notes. EQ.0: Parts not shown when dormant (flagged as “deleted”), EQ.1: Parts shown normally when dormant. NOPDEL Treatment of pressure loads on deleted elements, see notes. EQ.0: Pressure loads automatically deleted, EQ.1: No automatic deletion. Remarks: See also *DEFINE_CONSTRUCTION_STAGES and *DEFINE_STAGED_CONSTRUC- TION_PART. The staged construction options offer flexibility to carry out the whole construction simulation in one analysis, or to run it stage by stage. Provided that at least one construction stage is defined (*DEFINE_CONSTRUCTION_STAGES), a dynain file will be written at the end of each stage (file names are end_stage001_dynain, etc). These contain node and element definitions and the stress state; the individual stages can then be re-run without re-running the whole analysis. To do this, make a new input file as follows: • Copy the original input file, containing *DEFINE_CONSTRUCTION_- STAGES and *DEFINE_STAGED_CONSTRUCTION_PART. • Delete node and element definitions as these will be present in the dynain file (*NODE, *ELEMENT_SOLID, *ELEMENT_SHELL, and *ELEMENT_BEAM). • Delete any *INITIAL cards; the initial stresses in the new analysis will be taken from the dynain file. • On *CONTROL_STAGED_CONSTRUCTION set STGS to start at the desired stage • Add an *INCLUDE statement referencing, for example, end_stage002_dynain if starting the new analysis from Stage 3. • Move or copy the dynain file into the same directory as the new input file. When STGS is > 1 the analysis starts at a non-zero time (the start of stage STGS). In this case a dynain file must be included to start the analysis from the stress state at the end of the previous stage. The end time for stage STGE overrides the termination time on *CONTROL_TERMINATION. A new dynain file will be written at the end of all stages from STGS to STGE. ACCEL and FACT are used with *STAGED_CONSTRUCTION_PART for simpler input definition of the parts present at different construction stages. If STGS > 1 and elements have been deleted in a previous stage, these elements will be absent from the new analysis and should not be referred to (e.g. *DATABASE_HISTO- RY_SOLID) in the new input file. TSTART can be used to set a non-zero start time (again, assuming a compatible dynain file is included). This option is used only if construction stages have not been defined. STREF allows the user to set a construction stage at the start of which displacements are considered to be zero – e.g. so that initial analysis stages that achieve a pre-construction equilibrium do not contribute to contour plots of displacement. The current coordinates are not modified, only the “initial geometry” coordinates in the d3plot file. If this analysis starts from a stage later than STREF, the reference geometry will be taken from the dynain file that was written at the end of the stage previous to STREF – this dynain file must be in the same directory as the current model for this process to occur. This feature is not available in MPP. DORDEL: By default, parts for which *DEFINE_STAGED_CONSTRUCTION_PART is defined are flagged as “deleted” in the d3plot file at time-states for which the part is not active (i.e. STGA has not yet been reached). Parts that are deleted because STGR has been reached are also flagged as “deleted”. When animating the results, the parts should appear as they become active and disappear as they are deleted. If DORDEL is non-zero, inactive parts (before STGA) are shown normally. The parts are still shown as deleted after STGR is reached. NOPDEL: By default, pressure load “segments” are automatically deleted by LS-DYNA if they share all four nodes with a deleted solid or shell element. In staged construction, the user may want to apply pressure load to the surface of an element (A) that is initially shared with an element (B), where B is deleted during the calculation. For example, B may be in a layer of soil that is excavated, leaving A as the new top surface. The default scheme would delete the pressure segment when B is removed, despite the fact that A is still present. NOPDEL instructs LS-DYNA to skip the automatic deletion of pressure segments, irrespective of whether the elements have been deleted due to staged construction or material failure. The user must then ensure that pressure loads are not applied to nodes no longer supported by an active element. *CONTROL_STEADY_STATE_ROLLING Card 1 1 2 3 4 5 6 7 8 Variable IMASS LCDMU LCDMUR IVEL SCL_K Type Default I 0 I 0 I 0 I 0 I VARIABLE DESCRIPTION IMASS Inertia switching flag EQ.0: include inertia during an implicit dynamic simulation. EQ.1: treat steady state rolling subsystems as quasi-static during implicit dynamic simulations. LCDMU Optional load curve for scaling the friction forces in contact. LCDMUR Optional load curve for scaling the friction forces in contact during dynamic relaxation. If LCDMUR isn’t specified, LCDMU is used. IVEL Velocity switching flag. EQ.0: eliminate the steady state rolling body forces and set the velocities of the nodes after dynamic relaxation. EQ.1: keep the steady state rolling body forces after dynamic relaxation instead of setting the velocities. Scale factor for the friction stiffness during contact loading and unloading. The default values are 1.0 and 0.01 for explicit and implicit, respectively. Any scaling applied here applies only to contact involving the subsystem of parts defined for steady state rolling. SCL_K Remarks: 1. Treating the steady state rolling subsystems as quasi-static during an implicit simulation may eliminate vibrations in the system that are not of interest and is generally recommended. 2. Ramping up the friction by scaling it with LCDMU and LCDMUR may improve the convergence behavior of implicit calculations. The values of the load curves should be 0.0 at initial contact and ramp up smoothly to a value of 1.0. 3. After dynamic relaxation, the default behavior is to initialize the nodes with the velocities required to generate the body forces on elements and remove the body forces. This initialization is skipped, and the body forces retained, after dynamic relaxation if IVEL = 1. 4. The friction model in contact is similar to plasticity, where there is an elastic region during the loading and unloading of the friction during contact. The elastic stiffness is scaled from the normal contact stiffness. For implicit calcula- tions, the default scale factor is 0.01, which results in long periods of time being required to build the friction force, and, in some cases, oscillations in the contact forces. A value between 10 and 100 produces smoother solutions and a faster build-up and decay of the friction force as the tire velocity or slip angle is var- ied, allowing a parameter study to be performed in a single run. *CONTROL_STRUCTURED_{OPTION} Available options include: <BLANK> TERM Purpose: Write out an LS-DYNA structured input deck that is largely or wholly equivalent to the keyword input deck. This option may be useful in debugging errors that occur during processing of the input file, particularly if error messages of the type “*** ERROR ##### (STR + ###)” are written. The name of the structured input deck is “dyna.str”. Not all LS-DYNA features are supported in structured input format. Some data such as load curve numbers will be output in an internal numbering system. If the TERM option is activated, termination will occur after the structured input deck is written. Adding “outdeck = s” to the LS-DYNA execution line serves the same purpose as including *CONTROL_STRUCTURED in the keyword input deck. *CONTROL_SUBCYCLE_{K}_{L} or *CONTROL_SUBCYCLE_{OPTION} Available options for subcycling first form with K and L 𝐾, 𝐿 ∈ {<BLANK>, 1, 2, 4, 8, 16, 32, 64} Available options for multiscale (OPTION) include: <BLANK> MASS_SCALED_PART MASS_SCALED_PART_SET Purpose: This keyword is used to activate subcycling or mass scaling (multiscale). The common characteristic of both methods is that the time step varies from element to element, thereby eliminating unnecessary stepping on more slowly evolving portions of the model. These techniques are suited for reducing the computational cost for models involving large spatial variation in mesh density and/or material characteristics. Subcycling is described in the LS-DYNA Theory Manual and in detail in Borrvall et.al. [2014] and may be seen as an alternative to using selective mass scaling, see the keyword *CONTROL_TIMESTEP. This keyword comes in two variations: 1. Subcycling. Plain subcycling is activated by the *CONTROL_SUBCYCLE_{𝐾}_ {𝐿} variant of this keyword. This form of the card should not be included more than once. It may be used in conjunction with mass scaling to limit the time step characteristics. For subcycling, time steps for integration are determined automatically from the characteristic properties of the elements in the model, with the restriction that the ratio between the largest and smallest time step is limited by 𝐾. Fur- thermore, 𝐿 determines the relative time step at which external forces such as contacts and loads are calculated For example, *CONTROL_SUBCYCLE_16_4 limits the largest explicit integra- tion time step to at most 16 times the smallest. Contact forces are evaluated every 4 time steps. The defaults are 𝐾 = 16 and 𝐿 = 1, and L cannot be speci- fied larger than 𝐾. This option may be used without mass scaling activated but internally elements may still be slightly mass scaled to maintain computational efficiency. 2. Mass Scaling/Multiscale. For a multiscale simulation, mass scaling is mandatory and the time steps are directly specified in the input. The specified parts or part sets run at the time step specified in the TS field. All other elements evolve with a time step set by |DT2MS|, which is set on *CONTROL_TIMESTEP card. This feature was motivated by automotive crash simulation, wherein it is com- mon for a small subset of solid elements to limit the time step size. With this card the finely meshed parts (consisting of solid elements) can be made to run with a smaller time step through mass scaling so that the rest of the vehicle can run with a time step size of |DT2MS|. Part Card. Additional card for the MASS_SCALED_PART and MASS_SCALED_- PART_SET keyword options. Provide as many cards as necessary. Input ends at the next keyword (“*”) card. Card 1 1 2 3 4 5 6 7 8 Variable PID/PSID TS Type I F Default none none VARIABLE DESCRIPTION PID/PSID Part ID or part set ID if the SET option is specified. TS Time step size at which mass scaling is invoked for the PID or PSID Purpose: Stop the job. *CONTROL_TERMINATION Card 1 1 2 3 4 5 6 7 8 Variable ENDTIM ENDCYC DTMIN ENDENG ENDMAS NOSOL Type F Default 0.0 I 0 F F F 0.0 0.0 1.0E+08 I 0 Remarks 1 2 VARIABLE DESCRIPTION ENDTIM Termination time. Mandatory. ENDCYC DTMIN ENDENG ENDMAS Termination cycle. The termination cycle is optional and will be used if the specified cycle is reached before the termination time. Cycle number is identical with the time step number. Reduction (or scale) factor to determine minimum time step, tsmin, where tsmin= dtstart× DTMIN and dtstart is the initial step size determined by LS-DYNA. When the time step drops to tsmin, LS-DYNA terminates with a restart dump. See the exception described in Remark 2. Percent change in energy ratio for termination of calculation. If undefined, this option is inactive. Percent change in the total mass for termination of calculation. This option is relevant if and only if mass scaling is used to limit the minimum time step size, see *CONTROL_TIMESTEP variable name “DT2MS”. NOSOL Flag for a non-solution run, i.e. normal termination directly after initialization. EQ.0: off (default), EQ.1: on. Remarks: 1. Termination by displacement may be defined in the *TERMINATION section. 2. If the erosion flag on *CONTROL_TIMESTEP is set (ERODE = 1), then solid elements and thick shell elements whose time step falls below tsmin will be eroded and the analysis will continue. This time-step-based failure option is not recommended when solid formulations 11 or 12 are included in the model. Furthermore, when PSFAIL in *CONTROL_SOLID is nonzero, regardless of the value of ERODE, then all solid elements excepting those with formulation 11 or 12, whose time step falls below tsmin will be eroded and the analysis will con- tinue. This time-step-based erosion of solids due to a nonzero PSFAIL is not limited to solids in part set PSFAIL. Only the negative-volume-based erosion criterion is limited to solids in part PSFAIL. *CONTROL_THERMAL_EIGENVALUE Purpose: Compute eigenvalues of thermal conductance matrix for model evaluation purposes. Card 1 1 2 3 4 5 6 7 8 Variable NEIG Type Default I 0 . . VARIABLE DESCRIPTION NEIG Number of eigenvalues to compute. EQ.0: No eigenvalues are computed. GT.0: Compute NEIG eigenvalues of each thermal conductance matrix. Remarks: 1. Computes NEIG eigenvalues for each thermal conductance matrix. This is a model evaluation tool and it is recommended that only a small number, such as 1, thermal time steps are used when using this feature. *CONTROL_THERMAL_NONLINEAR Purpose: Set parameters for a nonlinear thermal or coupled structural/thermal analysis. The control card, *CONTROL_SOLUTION, is also required. Card 1 1 2 3 4 5 6 7 8 Variable REFMAX TOL DCP LUMPBC THLSTL NLTHPR PHCHPN Type I F F Default 10 1.e-04 1.0 or 0.5 I 0 F 0. I 0 F 100. VARIABLE DESCRIPTION REFMAX Maximum number of matrix reformations per time step: EQ.0: set to 10 reformations. TOL Convergence tolerance for temperature: EQ.0.0: set to 1000 * machine roundoff. DCP Divergence control parameter: steady state problems 0.3 ≤ DCP ≤ 1.0 0.0 < DCP ≤ 1.0 transient problems default 1.0 default 0.5 LUMPBC Lump enclosure radiation boundary condition. LUMPBC = 1 activates a numerical method to damp out anomalous temperature oscillations resulting from very large step function boundary conditions. This option is not generally recommended. EQ.0: off (default) EQ.1: on THLSTL Line search convergence tolerance: EQ.0.0: No line search GT.0.0: Line search convergence tolerance VARIABLE DESCRIPTION NLTHPR Thermal nonlinear print out level: EQ.0: No print out EQ.1: Print convergence parameters during solution of nonlinear system PHCHPN Phase change penalty parameter: EQ.0.0: Set to default value 100. GT.0.0: Penalty to enforce constant phase change temperature *CONTROL Purpose: Set options for the thermal solution in a thermal only or coupled structural- thermal analysis. The control card, *CONTROL_SOLUTION, is also required. Card 1 1 2 3 4 5 6 7 8 Variable ATYPE PTYPE SOLVER CGTOL GPT EQHEAT FWORK SBC Type Default I 0 I 0 I F 3 10-4/10-6 I 8 F 1. F 1. Remaining cards are optional.† Card 2 1 2 3 4 5 6 7 Variable MSGLVL MAXITR ABSTOL RELTOL OMEGA Type Default I 0 I F F F 500 10-10 10-6 1.0 or 0. F 0. 8 TSF F 1. Card 3 1 2 3 4 5 6 7 8 Variable MXDMP DTVF VARDEN Type Default I 0 F 0. I 0 . *CONTROL_THERMAL_SOLVER Card 2 1 2 3 4 5 6 7 8 Variable MSGLVL NINNER ABSTOL RELTOL NOUTER Type Default I 0 I F F I 100 10-10 10-6 100 VARIABLE DESCRIPTION ATYPE Thermal analysis type: EQ.0: Steady state analysis, EQ.1: transient analysis. PTYPE Thermal problem type: EQ.0: linear problem, EQ.1: nonlinear problem with material properties evaluated at gauss point temperature. EQ.2: nonlinear problem with material properties evaluated at element average temperature. VARIABLE DESCRIPTION SOLVER Thermal analysis solver type: EQ.1: using solver 11 (enter -1 to use the old ACTCOL solver), EQ.2: nonsymmetric direct solver, EQ.3: diagonal scaled conjugate gradient iterative (default), EQ.4: incomplete choleski conjugate gradient iterative, EQ.5: nonsymmetric diagonal scaled bi-conjugate gradient EQ.11: symmetric direct solver For MPP executables: EQ.11: symmetric direct solver, EQ.12: diagonal scaling (default for mpp) conjugate gradient iterative, EQ.13: symmetric Gauss-Siedel conjugate gradient iterative, EQ.14: SSOR conjugate gradient iterative, EQ.15: ILDLT0 (incomplete factorization) conjugate gradient iterative, EQ.16: modified ILDLT0 (incomplete factorization) conjugate gradient iterative. For Conjugate Heat transfer problems: EQ.17: GMRES solver. CGTOL Convergence tolerance for SOLVER = 3 and 4. EQ.0.0: use default value 10−4 single or 10−6 double precision GPT Number of Gauss points to be used in the solid elements: EQ.0.0: use default value 8, EQ.1.0: one point quadrature is used. EQHEAT Mechanical equivalent of heat . EQ.0.0: default value 1.0, LT.0.0: designates a load curve number for EQHEAT versus time. FWORK Fraction of mechanical work converted into heat. EQ.0.0: use default value 1.0. SBC *CONTROL_THERMAL_SOLVER DESCRIPTION Stefan Boltzmann constant. radiation surfaces, see *BOUNDARY_RADIATION_… Value is used with enclosure LT.0.0: use a smoothing algorithm when calculating view factors to force the row sum = 1. MSGLVL Output message level (For SOLVER > 10) EQ.0: no output (default), EQ.1: summary information, EQ.2: detailed information, use only for debugging. MAXITR Maximum number of iterations. For SOLVER > 11. EQ.0: use default value 500, ABSTOL Absolute convergence tolerance. For SOLVER > 11. EQ.0.0: use default value 10−10 RELTOL Relative SOLVER > 11. convergence tolerance. Replaces CGTOL for EQ.0.0: use default value 10−6 OMEGA Relaxation parameter omega for SOLVER 14 and 16. TSF EQ.0.0: use default value 1.0 for Solver 14, use default value 0.0 for Solver 16. Thermal Speedup Factor. This factor multiplies all thermal parameters with units of time in the denominator (e.g., thermal conductivity, convection heat transfer coefficients). It is used to artificially time scale the problem. Its main use is in metal stamping. If the velocity of the stamping punch is artificially increased by 1000, then set TSF = 1000 to scale the thermal parameters. MXDMP Matrix Dumping for SOLVER > 11 EQ.0: No Dumping GT.0: Dump using ASCII format every MXDMP time steps. LT.0: Dump using binary format every |MXDMP| time steps. DTVF Time interval between view factor updates. VARIABLE VARDEN DESCRIPTION Variable thermal density. This parameter is only applicable for solid elements in a coupled thermal-stress problem. Setting this parameter will adjust the material thermal density in the thermal solver to account for very large volume changes when using an EOS or large coefficient of thermal expansion. For most applications, the default value, VARDEN = 0, should be used. EQ.0: use constant density (default) EQ.1: modify thermal density to account for volume change when using an EOS. EQ.2: modify thermal density to account for volume change when using a large coefficient of expansion. NINNER Number of inner iterations for GMRES solve NOUTER Number of outer iterations for GMRES solve Remarks: 1. Solver Availability in MPP. Solvers 1, 2, 3 and 4 are only for SMP environ- ments. Solvers 11, 12, 13, 14, 15 and 16 are for SMP and MPP. 2. Recommended Direct Solver. Solver 11 is the preferred direct solver. Solver 11 uses sparse matrix storage and requires much less memory than Solver 1. 3. Direct vs. Iterative Solve. Use of a direct solver (e.g., SOLVER = 1, 2 or 11) is usually less efficient than using an iterative solver (SOLVER = 3, 4, 12, 13, 14, 15 or 16). Consider using a direct solver to get the model running and then switch to an iterative solver to decrease execution time (particularly for large models). Direct solvers should be used when experiencing slow or no convergence. 4. Transient Problems. For transient problems, diagonal scaling conjugate gradient (SOLVER = 3 or 12) should be adequate. 5. Steady State Problems. For steady state problems, convergence may be slow or unacceptable, so consider using direct solver (SOLVER = 1, 2 or 11) or a more powerful preconditioner (SOLVER = 4, 13, 14, 15 or 16). 6. Solvers 13 & 14. Solver 13 (symmetric Gauss-Seidel) and solver 14 (SSOR) are related. When OMEGA = 1, solver 14 is equivalent to solver 13. The optimal omega value for SSOR is problem dependent but lies between 1 and 2. 7. Solvers 15 & 16. Solver 15 (incomplete LDLT0) and solver 16 (modified incomplete LDLT0) are related. Both are no-fill factorizations that require one extra n-vector of storage. The sparsity pattern of the preconditioner is exactly the same as that of the thermal stiffness matrix. Solver 16 uses the relaxation parameter OMEGA. The optimal OMEGA value is problem dependent, but lies between 0 and 1. 8. Solver 17. The GMRES solver has been developed as an alternative to the direct solvers in cases where the structural thermal problem is coupled with the fluid thermal problem in a monolithic approach using the ICFD solver. A sig- nificant gain of calculation time can be observed when the problem reaches 1M elements. 9. Completion Conditions for Solvers 12 – 15. Solvers 12, 13, 14, 15 and 16 terminate the iterative solution process when (1) the number of iterations ex- ceeds MAXITR or (2) the 2-norm of the residual drops below ABSTOL + RELTOL × 2-norm of the initial residual. 10. Debug Data. Solvers 11 and up have the ability to dump the thermal conductance matrix and right-hand-side using the same formats as documented under *CONTROL_IMPLICIT_SOLVER. If this option is used files beginning with “T_”will be generated. 11. Unit Conversion Factor. EQHEAT is a unit conversion factor. EQHEAT converts the mechanical unit for work into the thermal unit for energy accord- ing to, EQHEAT × [work] = [thermal energy] However, it is recommended that a consistent set of units be used with EQHEAT set to 1.0. For example when using SI, [work] = 1Nm = [thermal energy] = 1J ⇒ EQHEAT = 1. *CONTROL_THERMAL_TIMESTEP Purpose: Set time step controls for the thermal solution in a thermal only or coupled structural/thermal analysis. This card requires that the deck also include *CONTROL_- SOLUTION, and, *CONTROL_THERMAL_SOLVER needed. Card 1 Variable Type Default 1 TS I 0 2 TIP 3 4 5 6 7 8 ITS TMIN TMAX DTEMP TSCP LCTS F F 0.5 none F - F - F F 1.0 0.5 I 0 VARIABLE DESCRIPTION TS Time step control: EQ.0: fixed time step, EQ.1: variable time step (may increase or decrease). TIP Time integration parameter: EQ.0.0: set to 0.5 - Crank-Nicholson scheme, EQ.1.0: fully implicit. ITS Initial thermal time step TMIN Minimum thermal time step: EQ.0.0: set to structural explicit time step. TMAX Maximum thermal time step: EQ.0.0: set to 100 * structural explicit time step. DTEMP Maximum temperature change in each time step above which the thermal time step will be decreased: EQ.0.0: set to a temperature change of 1.0. TSCP Time step control parameter. The thermal time step is decreased by this factor if convergence is not obtained. 0. < TSCP < 1.0: EQ.0.0: set to a factor of 0.5. LCTS *CONTROL_THERMAL_TIMESTEP DESCRIPTION LCTS designates a load curve number which defines data pairs of (thermal time breakpoint, new time step). The time step will be adjusted to hit the time breakpoints exactly. After the time breakpoint, the time step will be set to the ‘new time step’ ordinate value in the load curve. *CONTROL Purpose: Set structural time step size control using different options. Card 1 1 2 3 4 5 6 7 8 Variable DTINIT TSSFAC ISDO TSLIMT DT2MS LCTM ERODE MS1ST Type F F Default - 0.9 or 0.67 I 0 F F 0.0 0.0 I 0 I 0 I 0 This card is optional. Card 2 1 2 3 4 5 6 7 8 Variable DT2MSF DT2MSLC IMSCL RMSCL Type F I Default not used not used I 0 F 0.0 VARIABLE DESCRIPTION DTINIT Initial time step size: EQ.0.0: LS-DYNA determines initial step size. TSSFAC Scale factor for computed time step (old name SCFT). See Remark 1 below. (Default = 0.90; if high explosives are used, the default is lowered to 0.67). ISDO *CONTROL_TIMESTEP DESCRIPTION Basis of time size calculation for 4-node shell elements. 3-node shells use the shortest altitude for options 0,1 and the shortest side for option 2. This option has no relevance to solid elements, which use a length based on the element volume divided by the largest surface area. EQ.0: characteristic length is given by area min(longest side, longest diagonal ) . EQ.1: characteristic length is given by area longest diagonal . EQ.2: based on bar wave speed and, max [shortest side, area min(longest side, longest diagonal ) ] . WARNING: Option 2 can give a much larger time step size that can lead to instabilities in some applications, especially when triangular elements are used. EQ.3: This feature is currently unavailable. Time step size is based on the maximum eigenvalue. This option is okay for structural applications where the material sound speed changes slowly. The cost related to determining the maximum eigenvalue is significant, but the increase in the time step size often allows for significantly shorter run times without using mass scaling. VARIABLE TSLIMT DESCRIPTION Shell element minimum time step assignment, TSLIMT. When a shell controls the time step, element material properties (moduli not masses) will be modified such that the time step does not fall below the assigned step size. This option is applicable only to shell elements using material models: *MAT_PLASTIC_KINEMATIC, *MAT_POWER_LAW_PLASTICITY, *MAT_STRAIN_RATE_DEPENDENT_PLASTICITY, *MAT_PIECE-WISE_LINEAR_PLASTICITY. WARNING: This so-called stiffness scaling option is NOT recommended. The DT2MS op- tion below applies to all materials and element classes and is preferred. If both TSLIMT and DT2MS below are active and if TSLIMT is input as a positive number, then TSLIMT defaults to 10−18, thereby disabling it. If TSLIMT is negative and less than |DT2MS|, then |TSLIMT| is applied prior to the mass being scaled. If |DT2MS| exceeds the magnitude of TSLIMT, then TSLIMT is set to 10−18. VARIABLE DESCRIPTION DT2MS Time step size for mass scaled solutions. (Default = 0.0) GT.0.0: Positive values are for quasi-static analyses or time history analyses where the inertial effects are insignifi- cant. LT.0.0: TSSFAC × |DT2MS| is the minimum time step size permitted and mass scaling is done if and only if it is necessary to meet the Courant time step size criterion. This option can be used in transient analyses if the mass increases remain insignificant. See also the varia- ble MS1ST below and the *CONTROL_TERMINA- TION variable ENDMAS. WARNING: Superelements from, *ELEMENT_DI- RECT_MATRIX_INPUT, are not mass scaled; consequently, DT2MS does not affect their time step size. In this case an error termination will occur, and DT2MS will need to be reset to a smaller value. LCTM Load curve ID that limits the maximum time step size (optional). This load curve defines the maximum time step size permitted versus time. If the solution time exceeds the final time value defined by the curve the computed step size is used. If the time step size from the load curve is exactly zero, the computed time step size is also used. VARIABLE DESCRIPTION ERODE Erosion flag for solids and thick shells. EQ.0: Calculation will terminate if time step drops to tsmin . EQ.1: Solids and thick shells whose time step drops to tsmin will erode, and SPH particles whose time step drops to tsmin will be deac- tivated. ERODE = 1 and tsmin > 0 also invokes erosion of any solid element whose volume becomes negative, thereby preventing termination of the analysis due to negative volume. The effect of ERODE = 1 on erosion due to negative volue is superceded by a nonzero PSFAIL in *CONTROL_SOLID. PSFAIL serves to limit solid erosion based on negative volume to solids in part set PS- FAIL. MS1ST Option for mass scaling that applies when DT2MS < 0. EQ.0: (Default) Mass scaling is considered throughout the analysis to ensure that the minimum time step cannot drop below TSSFAC × |DT2MS|. Added mass may in- crease with time, but it will never decrease. EQ.1: Added mass is calculated at the first time step and remains unchanged thereafter. The initial time step will not be less than TSSFAC × |DT2MS|, but the time step may subsequently decrease, depending on how the mesh deforms and the element characteristic lengths change. DT2MSF Reduction (or scale) factor for initial time step size to determine the minimum time step size permitted. Mass scaling is done if it is necessary to meet the Courant time step size criterion. If this option is used, DT2MS effectively becomes –DT2MSF multiplied by the initial time step size, Δ𝑡, before Δ𝑡 is scaled by TSSFAC. This option is active if and only if DT2MS = 0 above. DT2MSLC *CONTROL_TIMESTEP DESCRIPTION Load curve for determining the magnitude of DT2MS as a function of time, 𝑓DT2MS(𝑡), during the explicit solutions phase. Time zero must be in the abscissa range of this curve and the ordinate values should all be positive. At a given simulation time 𝑡, 𝑓DT2MS(𝑡) × sign(DT2MS) plays the role of DT2MS according to the description for DT2MS above. It is allowed to use all negative ordinate values in the curve, then 𝑓DT2MS(𝑡) itself (sign and magnitude) determines how mass scaling is performed and DT2MS is neglected. It is however not allowed for the ordinate values to change sign during the simulation. IMSCL Flag for selective mass scaling if and only if mass scaling active. Selective mass scaling does not scale the rigid body mass and is therefore more accurate. Since it is memory and CPU intensive, it should be applied only to small finely meshed parts. EQ.0: no selective mass scaling. EQ.1: all parts undergo selective mass scaling. LT.0: recommended: |IMSCL| is the part set ID of the parts that undergo selective mass scaling; all other parts are mass scaled the usual way. RMSCL Flag for using rotational option in selective mass scaling EQ.0.: Only translational inertia are selectively mass scaled NE.0.: Both translational and rotational inertia are selectively mass scaled Remarks: During the solution we loop through the elements and determine a new time step size by taking the minimum value over all elements. Δ𝑡 𝑛+1 = TSSFAC × min{Δ𝑡1, Δ𝑡2, . . . , Δ𝑡𝑁} where N is the number of elements. The time step size roughly corresponds to the transient time of an acoustic wave through an element using the shortest characteristic distance. For stability reasons the scale factor TSSFAC is typically set to a value of 0.90 (default) or some smaller value. To decrease solution time we desire to use the largest possible stable time step size. Values larger than .90 will often lead to instabilities. Some comments follow: 1. Sound Speed and Element Size. The sound speed in steel and aluminum is approximately 5mm per microsecond; therefore, if a steel structure is modeled with element sizes of 5mm, the computed time step size would be 1 microsec- ond. Elements made from materials with lower sound speeds, such as foams, will give larger time step sizes. Avoid excessively small elements and be aware of the effect of rotational inertia on the time step size in the Belytschko beam element. Sound speeds differ for each material, for example, consider: Air Water Steel Titanium Plexiglass 331 m/s 1478 5240 5220 2598 2. Use Rigid Bodies when Possible. It is recommended that stiff components be modeled by using rigid bodies. Do not scale the Young’s modulus, as that can substantially reduce the time step size. 3. Triangular Elements. The altitude of the triangular element should be used to compute the time step size. Using the shortest side is okay only if the calcula- tion is closely examined for possible instabilities. This is controlled by parame- ter ISDO. 4. Selective Mass Scaling. In the explicit time integration context and in contrast to conventional mass scaling, selective mass scaling (SMS) is a well thought out scheme that not only reduces the number of simulation cycles but that also does not significantly affect the dynamic response of the system under consideration. The drawback is that a linear system of equations must be solved in each time step for the accelerations. In this implementation a pre- conditioned conjugate gradient method (PCG) is used. An unfortunate consequence of this choice of solver is that the efficiency will worsen when attempting large time steps since the condition number of the assembled mass matrix increases with the added mass. Therefore caution should be taken when choosing the desired time step size. For large models it is also recommended to only use SMS on critical parts since it is otherwise like- ly to slow down execution; the bottleneck being the solution step for the sys- tem of linear system of equations. While some constraints and boundary conditions available in LS-DYNA are not supported for SMS they can be implemented upon request from a user. A partial list of constraints and boundary conditions supported with SMS: Pointwise nodal constraints in global and local directions Prescribed motion in global and local directions Adaptivity Rigid walls Deformable elements merged with rigid bodies Constraint contacts and spotwelds Beam release constraints By default, only the translational dynamic properties are treated. This means that only rigid body translation will be unaffected by the mass scaling imposed. There is an option to also properly treat rigid body rotation in this way, this is invoked by flagging the parameter RMSCL. A penalty in computational ex- pense is incurred but the results could be improved if rotations are dominating the simulation. *CONTROL Purpose: Specify the user units for the current keyword input deck. This does not provide any mechanism for automatic conversion of units of any entry in the keyword input deck. It is intended to be used for several purposes, but currently only for the situation where an external database in another set of units will be loaded and used in the simulation. In this case, *CONTROL_UNITS provides the information necessary to convert the external data into internal units . If the needed unit is not one of the predefined ones listed for use on the first card, then the second optional card is used to define that unit. Any non-zero scales that are entered on optional card 2 override what is specified on the first card. These scales are given in terms of the default units on card 1. For instance, if 3600.0 is given in the second 20 character field on the optional second card (TIME_SCALE), then ‘hour’ is the time unit (3600 seconds). Card 1 1 2 3 4 5 6 7 8 Variable LENGTH TIME MASS TEMP Type A A A Default m sec kg A K Optional Card only used when a new unit needs to be defined: Card 2 1 2 3 4 5 6 7 8 Variable LENGTH_SCALE TIME_SCALE MASS_SCALE Type F Default 1.0 F 1.0 F 1.0 VARIABLE DESCRIPTION LENGTH Length units: EQ.m: meter (default) EQ.mm: millimeter EQ.cm: centimeter EQ.in: inch EQ.ft: foot TIME Time units: EQ.sec: EQ.ms: second (default) msec, millisec EQ.micro_s: microsec MASS Mass units: EQ.kg: EQ.g: EQ.mg: EQ.lb: kilogram (default) gram milligram pound EQ.slug: pound × sec2/foot EQ.slinch: pound × sec2/inch EQ.mtrc_ton: metric_ton TEMP Temperature units: EQ.K: Kelvin (default) EQ.C: Celsius EQ.F: Fahrenheit EQ.R: Rankine LENGTH_ SCALE TIME_ SCALE MASS_ SCALE Number of meters in the length unit for the input deck Number of seconds in the time unit for the input deck Number of kilograms in the mass unit for the input deck The Keyword options in this section in alphabetical order are: *DAMPING_FREQUENCY_RANGE_{OPTION} *DAMPING_GLOBAL *DAMPING_PART_MASS *DAMPING_PART_STIFFNESS *DAMPING_RELATIVE *DAMPING_FREQUENCY_RANGE_{OPTION} Purpose: This feature provides approximately constant damping (i.e. frequency- independent) over a range of frequencies. Available OPTIONS are: <BLANK> Applies damping to global motion DEFORM Applies damping to element deformation Card 1 1 2 3 4 5 6 7 8 Variable CDAMP FLOW FHIGH PSID (blank) PIDREL IFLG Type F F F Default 0.0 0.0 0.0 I 0 I 0 I 0 VARIABLE DESCRIPTION CDAMP Damping in fraction of critical. FLOW FHIGH PSID PIDREL Lowest frequency in range of interest (cycles per unit time, e.g. Hz if time unit is seconds) Highest frequency in range of interest (cycles per unit time, e.g. Hz if time unit is seconds) Part set ID. The requested damping is applied only to the parts in the set. If PSID = 0, the damping is applied to all parts except those referred to by other *DAMPING_FREQUENCY_RANGE cards. Optional part ID of rigid body. Damping is then applied to the motion relative to the rigid body motion. This input does not apply to the DEFORM option. IFLG Method used for internal calculation of damping constants: EQ.0: Iterative (more accurate), EQ.1: Approximate (same as R9 and previous versions). Remarks: This feature provides approximately constant damping (i.e. frequency-independent) over a range of frequencies. 𝐹low < 𝐹 < 𝐹highIt is intended for small damping ratios (e.g. < 0.05) and frequency ranges such that 𝐹high/𝐹low is in the range 10 to 300. The drawback to this method of damping is that it reduces the dynamic stiffness of the model, especially at low frequencies. Where the model contains, for example, a rigid foundation or base, the effects of this stiffness reduction can be ameliorated by using PIDREL. In this case, the damping forces resist motion relative to the base, and are reacted onto the rigid part PIDREL. “Relative motion” here means the difference between the velocity of the node being damped, and the velocity of a point rigidly connected to PIDREL at the same coordinates as the node being damped. This effect is predictable: the natural frequencies of modes close to 𝐹low are reduced by 3% for a damping ratio of 0.01 and 𝐹high/𝐹low in the range 10-30. Near 𝐹high the error is between zero and one third of the error at 𝐹low. Estimated frequency errors are shown in the next table. Damping Ratio 0.01 0.02 0.04 % error for Fhigh/Flow = 3 to 30 30 to 300 300 to 3000 3% 6% 12% 4.5% 9% 18% 6% 12% 24% It is recommended that the elastic stiffnesses in the model be increased slightly to account for this, e.g. for 0.01 damping across a frequency range of 30 to 600Hz, the average error across the frequency range is about 2%. Increase the stiffness by (1.02)2, i.e. by 4%. Starting from R10, an iterative method is used for the internal calculation of the damping constants . The new method results in the actual damping matching the user-input damping ratio CDAMP more closely across the frequency range FLOW to FHIGH. As an example, for CDAMP = 0.01, FLOW = 1 Hz and FHIGH = 30 Hz, the actual damping achieved by the previous approximate method varied between 0.008 and 0.012 (different values at different frequencies), i.e. there were errors of up to 20% of the target CDAMP. With the iterative algoritm, the errors are reduced to 1% of the target CDAMP. *DAMPING_FREQUENCY_RANGE The DEFORM option applies damping to the element responses (unlike the standard *DAMPING_FREQUENCY_RANGE which damps the global motion of the nodes). Therefore, rigid body motion is not damped when the DEFORM keyword option is used. For this reason, DEFORM is recommended over the standard option. The damping is adjusted based on current tangent stiffness; this is believed to be more appropriate for a nonlinear analysis, which could be over-damped if a strain-rate- proportional or viscous damping scheme were used. It works with the following element formulations: • Solids – types -1, -2, 1, 2, 3, 4, 9, 10, 13, 15, 16, 17, 99 • Beams – types 1, 2, 3, 4, 5, 9 (note: not type 6) • Shells – types 1-5, 7-17, 20, 21, 23-27, 99 • Discrete elements The DEFORM option differs from the standard option in several ways: Standard Damping vs. Deformation Damping Characteristic Property Keyword Option <BLANK> DEFORM Damping on Node velocities Element responses Rigid body motion Can be damped Never damped Natural frequencies Reduced (by percentages shown in the above table) Increased (percentages shown in the above table) Recommended compensation Increase elastic stiffness Reduce elastic stiffness Effect on timestep None Small reduction applied automatically, same percentage as in the frequency change Element types damped All See list above Damping energy output Included in “system damping energy” Included in Internal Energy only if RYLEN = 2 on *CON- TROL_ENERGY *DAMPING Purpose: Define mass weighted nodal damping that applies globally to the nodes of deformable bodies and to the mass center of the rigid bodies. For specification of mass damping by part ID or part set ID, use *DAMPING_PART_MASS. Card 1 1 2 3 4 5 6 7 8 Variable LCID VALDMP STX STY STZ SRX SRY SRZ Type Default Remarks I 0 1 VARIABLE LCID F F F F F F F 0.0 0.0 0.0 0.0 0.0 0.0 0.0 2 2 2 2 2 2 DESCRIPTION Load curve ID which specifies the system damping constant vs. time: EQ.0: a constant damping factor as defined by VALDMP is used, GT.0: system damping is given by load curve LCID (which must be an integer). The damping force applied to each node is 𝑓 = −𝑑(𝑡)𝑚𝑣, where 𝑑(𝑡) is defined by load curve LCID. VALDMP System damping constant, Ds (this option is bypassed if the load curve number defined above is non zero). STX STY STZ SRX SRY SRZ Scale factor on global 𝑥 translational damping forces. Scale factor on global 𝑦 translational damping forces. Scale factor on global 𝑧 translational damping forces. Scale factor on global 𝑥 rotational damping moments. Scale factor on global 𝑦 rotational damping moments. Scale factor on global 𝑧 rotational damping moments. *DAMPING_GLOBAL 1. Restart. This keyword is also used for the restart, see *RESTART. 2. Defaults for Scale Factors. If STX = STY = STZ = SRX = SRY = SRZ = 0.0 in the input above, all six values are defaulted to unity. 3. Damping Exceptions. Mass damping will not be applied to deformable nodes with prescribed motion or to nodes tied with CONSTRAINED_NODE_SET. 4. Formulation. With mass proportional system damping the acceleration is computed as: 𝐚𝑛 = 𝐌−1(𝐏𝑛 − 𝐅𝑛 − 𝐅damp where, 𝐌 is the diagonal mass matrix, 𝐏𝐧 is the external load vector, 𝐅𝑛 is the internal load vector, and 𝐅damp is the force vector due to system damping. This latter vector is defined as: ) 𝐅damp = 𝐷𝑠𝑚𝐯 The best damping constant for the system is usually some value approaching the critical damping factor for the lowest frequency mode of interest. (𝐷𝑠)critical = 2𝜔min The natural frequency 𝜔min (given in radians per unit time) is generally taken as the fundamental frequency of the structure. This frequency can be determined from an eigenvalue analysis or from an undamped transient analysis. Note that this damping applies to both translational and rotational degrees of freedom. Also note that mass proportional damping will damp rigid body motion as well as vibration. Energy dissipated by through mass weighted damping is reported as system damping energy in the ASCII file glstat. This energy is computed whenever system damping is active. *DAMPING OPTION specifies that a part set ID is given with the single option: <BLANK> SET If not used a part ID is assumed. Purpose: Define mass weighted damping by part ID. Parts may be either rigid or deformable. In rigid bodies the damping forces and moments act at the center of mass. This command may appear multiple times in an input deck but cannot be combined with *DAMPING_GLOBAL. Card 1 1 2 Variable PID/PSID LCID Type Default I 0 I 0 3 SF F 1.0 4 5 6 7 8 FLAG I 0 Scale Factor Card. Additional Card for FLAG = 1. Card 2 1 2 3 4 5 6 7 8 Variable STX STY STZ SRX SRY SRZ Type F F F F F F Default 0.0 0.0 0.0 0.0 0.0 0.0 VARIABLE DESCRIPTION PID/PSID Part ID, see *PART or part set ID, see *SET_PART. LCID Load curve ID which specifies the damping constant vs. time, applied to the part(s) specified in PID/PSID. VARIABLE DESCRIPTION Scale factor for load curve. This allows a simple modification of the load curve values. Set this flag to unity if the global components of the damping forces require separate scale factors. Scale factor on global 𝑥 translational damping forces. Scale factor on global 𝑦 translational damping forces. Scale factor on global 𝑧 translational damping forces. Scale factor on global 𝑥 rotational damping moments. Scale factor on global 𝑦 rotational damping moments. Scale factor on global 𝑧 rotational damping moments. SF FLAG STX STY STZ SRX SRY SRZ Remarks: Mass weighted damping damps all motions including rigid body motions. For high frequency oscillatory motion stiffness weighted damping may be preferred. With mass proportional system damping the acceleration is computed as: 𝛂𝑛 = 𝐌−1(𝐏𝑛 − 𝐅𝑛 − 𝐅damp where, 𝐌 is the diagonal mass matrix, 𝐏𝑛 is the external load vector, 𝐅𝑛 is the internal is the force vector due to system damping. This latter vector is load vector, and 𝐅damp defined as: ) 𝐅damp = 𝐷𝑠𝑚𝝂 The critical damping constant for the lowest frequency mode of interest is 𝐷𝑠 = 2𝜔min where 𝜔min is that lowest frequency in units of radians per unit time. The damping constant specified as the ordinate of curve LCID is typically less than the critical damping constant. The damping is applied to both translational and rotational degrees of freedom. The component scale factors can be used to limit which global components see damping forces. Energy dissipated by through mass weighted damping is reported as system damping energy in the ASCII file glstat. This energy is computed whenever system damping is active. Mass damping will not be applied to deformable nodes with prescribed motion or to nodes tied with CONSTRAINED_NODE_SET. *DAMPING_PART_STIFFNESS_{OPTION} OPTION specifies that a part set ID is given with the single option: <BLANK> SET If the SET option is not used, a part ID goes in the first field of Card 1. Purpose: Assign Rayleigh stiffness damping coefficient by part ID or part set ID. This damping command does not apply to parts comprised of discrete elements (*ELE- MENT_DISCRETE) or discrete beams (*ELEMENT_BEAM with ELFORM = 6). Card 1 1 2 3 4 5 6 7 8 Variable PID/PSID COEF Type I F Default none 0.0 VARIABLE DESCRIPTION PID/PSID Part ID or part set ID . COEF Rayleigh damping coefficient. Two methods are now available: LT.0.0: Rayleigh damping coefficient in units of time, set based on a given frequency and applied uniformly to each el- ement in the specified part or part set. See remarks be- low. EQ.0.0: Inactive. GT.0.0: Rayleigh damping coefficient for stiffness weighted damping. Values between 0.01 and 0.25 are recom- mended. Higher values are strongly discouraged, and values less than 0.01 may have little effect. The damp- ing coefficient is uniquely defined for each element of the part ID. Remarks: The damping matrix in Rayleigh damping is defined as: 𝐂 = 𝛼𝐌 + 𝛽𝐊 where 𝐂, 𝐌, and 𝐊 are the damping, mass, and stiffness matrices, respectively. The constants α. and β are the mass and stiffness proportional damping constants. The mass proportional damping can be treated by system damping, see keywords: *DAMP- ING_GLOBAL and DAMPING_PART_MASS. Transforming 𝐂 with the ith eigenvector 𝛟𝑖 gives: 𝛟𝑖 T𝐂𝛟𝑖 = 𝛟𝑖 T(𝛼𝐌 + 𝛽𝐊)𝛟𝑖 = 𝛼 + 𝛽𝜔𝑖 2 = 2𝜔𝑖𝜉𝑖𝛿𝑖𝑗 where 𝜔𝑖 is the ith frequency (radians/unit time) and 𝜉𝑖 is the corresponding modal damping parameter. Generally, the stiffness proportional damping is effective for high frequencies and is orthogonal to rigid body motion. Mass proportional damping is more effective for low frequencies and will damp rigid body motion. If a large value of the stiffness based damping coefficient is used, it may be necessary to lower the time step size significantly. This must be done manually by reducing the time step scale factor on the *CONTROL_TIMESTEP control card. Since a good value of β is not easily identified, the coefficient, COEF, is defined such that a value of .10 roughly corresponds to 10% damping in the high frequency domain. In LS-DYNA versions prior to 960 or if COEF is input as less than 0, the critical damping coefficient is equal to 2 divided by 𝜔𝑖. For example, 10% of critical damping in the ith mode corresponds to 𝛽 = 0.20 𝜔𝑖 and COEF would be input as -𝛽. Typically, this method of applying stiffness damping is stable only if 𝛽 is significantly smaller than the explicit time step size. Energy dissipated by Rayleigh damping is computed if and only if the flag, RYLEN, on the control card, *CONTROL_ENERGY is set to 2. This energy is accumulated as element internal energy and is included in the energy balance. In the glstat file this energy will be lumped in with the internal energy. NOTE: Type 2 beam elements are a special case in which COEF is internally scaled by 0.1. Thus there is a factor of 10 less damping than stated above. This applies to both negative and positive values of COEF. *DAMPING_RELATIVE Purpose: Apply damping relative to the motion of a rigid body. For example, it could damp the deformation of a rotating tire relative to the wheel without damping the rotating motion. Card 1 1 2 3 4 5 6 7 8 Variable CDAMP FREQ PIDRB PSID DV2 LCID Type Default F 0 F 0 F 0 I 0 F 0.0 I 0 VARIABLE DESCRIPTION CDAMP Fraction of critical damping. Frequency at which CDAMP is to apply (cycles per unit time, e.g. Hz if time unit is seconds). Part ID of rigid body, see *PART. Motion relative to this rigid body will be damped. Part set ID. The requested damping is applied only to the parts in the set. Optional constant for velocity-squared term. See remarks. ID of curve that defines fraction of critical damping vs. time. CDAMP will be ignored if LCID is non-zero. FREQ PIDRB PSID DV2 LCID Remarks: 1. This feature provides damping of vibrations for objects that are moving through space. The vibrations are damped, but not the rigid body motion. This is achieved by calculating the velocity of each node relative to that of a rigid body, and applying a damping force proportional to that velocity. The forces are reacted onto the rigid body such that overall momentum is conserved. It is intended that the rigid body is embedded within the moving object. 2. Vibrations at frequencies below FREQ are damped by more than CDAMP, while those at frequencies above FREQ are damped by less than CDAMP. It is recommended that FREQ be set to the frequency of the lowest mode of vibra- tion. 3. The damping force of each node is calculated as follows: F = - (D . m . v) – (DV2 . m .v2). Where: D = 4π . CDAMP . FREQ m = mass of the node v = velocity of node relative to the velocity of a point on the rigid body at the same coordinates as the node. The database definitions are optional, but are necessary to obtain output files containing results information. In this section the database keywords are defined in alphabetical order: *DATABASE_OPTION *DATABASE_ALE *DATABASE_ALE_MAT *DATABASE_BINARY_OPTION *DATABASE_BINARY_D3PROP *DATABASE_CPM_SENSOR *DATABASE_CROSS_SECTION_OPTION1_{OPTION2} *DATABASE_EXTENT_OPTION *DATABASE_FATXML *DATABASE_FORMAT *DATABASE_FREQUENCY_ASCII_OPTION *DATABASE_FREQUENCY_BINARY_OPTION *DATABASE_FSI *DATABASE_FSI_SENSOR *DATABASE_HISTORY_OPTION *DATABASE_MASSOUT *DATABASE_NODAL_FORCE_GROUP *DATABASE_PROFILE *DATABASE_PAP_OUTPUT *DATABASE_PWP_FLOW *DATABASE_PWP_OUTPUT *DATABASE_RECOVER_NODE *DATABASE_SPRING_FORWARD *DATABASE_SUPERPLASTIC_FORMING *DATABASE_TRACER *DATABASE_TRACER_GENERATE The ordering of the database definition cards in the input file is completely arbitrary. *DATABASE OPTION1 specifies the type of database. LS-DYNA will not create an ASCII database unless the corresponding *DATABASE_OPTION1 card is included in the input deck. OPTION1 may be any of the items in the following list: ABSTAT Airbag statistics. ATDOUT Automatic tiebreak damage statistics for *CONTACT_AUTOMAT- IC_ONE_WAY_SURFACE_TO_SURFACE_TIEBREAK, OPTIONs 7, 9, 10, and 11 (only SMP at the moment). AVSFLT AVS database. See *DATABASE_EXTENT_OPTION. BEARING *ELEMENT_BEARING force output. BNDOUT Boundary condition forces and energy CURVOUT Output from *DEFINE_CURVE_FUNCTION. DEFGEO Deformed geometry file. (Note that to output this file in Chrysler format insert the following line in your .cshrc file: “setenv LSTC_ DEFGEO chrysler”) The nasbdf file (NASTRAN Bulk Data) is creat- ed whenever the DEFGEO file is requested. DCFAIL Failure function data for *MAT_SPOTWELD_DAIMLERCHRYSLER DEFORC Discrete spring and damper element (*ELEMENT_DISCRETE) data. If the user wishes to be selective about which discrete elements are output in deforc, use *DATABASE_HISTORY_DISCRETE_OPTION to select elements for output (but only if BEAM = 0 in *DATA- BASE_BINARY_D3PLOT) or set PF = 1 in *ELEMENT_DISCRETE to turn off output for particular elements; otherwise all discrete ele- ments are output. DEMASSFLOW Measure mass flow rate across defined plane and use together with *DEFINE_DE_MASSFLOW_PLANE. DISBOUT Discrete beam element, type 6, relative displacements, rotations, and force resultants, all in the local coordinate system, which is also out- put. Use with *DATABASE_HISTORY_BEAM. ELOUT Element data. See *DATABASE_HISTORY_OPTION. Also, see Card 3 of the *DATABASE_EXTENT_BINARY parameters INTOUT and NODOUT. This latter option will output all integration point data or extrapolated data to the connectivity nodes in a file call eloutdet. GCEOUT Geometric contact entities. GLSTAT Global data. Always obtained if ssstat file is activated. H3OUT Hybrid III rigid body dummies. JNTFORC Joint force file MATSUM Material energies. See Remarks 1 and 2 below. MOVIE MPGS See MOVIE option of *DATABASE_EXTENT_OPTION. See MPGS option of *DATABASE_EXTENT_OPTION. NCFORC Nodal interface forces. See *CONTACT - Card 1 (SPR and MPR) NODFOR Nodal force groups. See *DATABASE_NODAL_FORCE_GROUP. NODOUT Nodal point data. See *DATABASE_HISTORY_NODE_OPTION. PBSTAT Particle blast data. See *PARTICLE_BLAST PLLYOUT Pulley element data for *ELEMENT_BEAM_PULLEY. PRTUBE Pressure tube data for *DEFINE_PRESSURE_TUBE. RBDOUT Rigid body data. See Remark 2 below. RCFORC Resultant interface forces. Output in a local coordinate system is available, see *CONTACT, Optional Card C. RWFORC Wall forces. SBTOUT Seat belt output file SECFORC Cross section forces. See *DATABASE_CROSS_SECTION_OPTION. SLEOUT Sliding interface energy. See *CONTROL_ENERGY SPCFORC SPC reaction forces. SPHOUT SPH data. See *DATABASE_HISTORY_OPTION. SSSTAT Subsystem data. See *DATABASE_EXTENT_SSSTAT. SWFORC Nodal constraint reaction forces (spot welds and rivets). TPRINT Thermal output from a coupled structural/thermal or thermal only analysis. Includes all nodes unless *DATABASE_HISTORY_- NODE_OPTION is also provided in the keyword input. TRHIST Tracer particle history information. See *DATABASE_TRACER. OPTION2, if it set, must be set to FILTER, and this can only be used when OPTION1 is set to NCFORC. When set to FILTER the keyword requires an additional data card, see Card 2 below. To include global and subsystem mass and inertial properties in the glstat and ssstat files add the keyword option MASS_PROPERTIES as show below. If this option is active the current mass and inertia properties are output including the principle inertias and their axes. Mass of deleted nodes and rigid bodies are not included in the calculated properties. GLSTAT_MASS_PROPERTIES SSSTAT_MASS_PROPERTIES This is an option for the glstat file to include mass and inertial properties. This is an option for the ssstat file to include mass and inertial properties for the subsystems. Card 1 Variable 1 DT 2 3 4 5 6 7 8 BINARY LCUR IOOPT OPTION1 OPTION2 OPTION3 OPTION4 Type F I I I F/I Default 0. 1 or 2 none 0. 0 I 0 I 0 I 0 VARIABLE DT DESCRIPTION Time interval between outputs. If DT is zero, no output is printed. BINARY Flag for binary output. See remarks under "Output Files and Post-Processing" in Appendix O, “LS-DYNA MPP User Guide.” EQ.1: ASCII file is written: This is the default for shared memory parallel (SMP) LS-DYNA executables. EQ.2: Data written to a binary database “binout”, which contains data that would otherwise be output to the ASCII file. The ASCII file in this case is not created. This is the default for MPP LS-DYNA executables. EQ.3: ASCII file is written and the data is also written to the binary database (NOTE: MPP LS-DYNA executables will only produce the binary database). Optional curve ID specifying time interval between dumps. Use *DEFINE_CURVE to define the curve; abscissa is time and ordinate is time interval between dumps. Flag to govern behavior of the plot frequency load curve defined by LCUR: EQ.1: At the time each plot is generated, the load curve value is added to the current time to determine the next plot time.(this is the default behavior) EQ.2: At the time each plot is generated, the next plot time, 𝑡, is LCUR IOOPT VARIABLE DESCRIPTION computed so that 𝑡 = the current time + LCUR(𝑡) . EQ.3: A plot is generated for each abscissa point in the load curve definition. The actual value of the load curve is ignored. OPTION1 applies to either the bndout, nodout or elout files. For the nodout file OPTION1 is a real variable that defines the time interval between outputs for the high frequency file, nodouthf. If OPTION1 is zero, no output is printed. Nodal points that are to be output at a higher frequency are flagged using HFO in the DATABASE_HISTORY_NODE_LOCAL input. For the elout file OPTION1 is an integer variable that gives the number of additional history variables written into the elout file for each integration point in the solid elements. See Remark 7 below for the elout file and Remark 9 for the bndout file. OPTION2 applies to either the bndout, nodouthf or elout files. For the nodouthf OPTION2 defines the binary file flag for the high frequency nodouthf file. See BINARY above. For the elout file OPTION2 is an integer variable that gives the number of additional history variables written into the elout file for each integration point in the shell elements. See Remark 7 below for the elout file and Remark 9 for the bndout file. OPTION3 applies to the bndout and elout files only. For the elout file OPTION3 is an integer variable that gives the number of additional history variables written into the elout file for each integration point in the thick shell elements. See Remark 7 below for the elout file and Remark 9 for the bndout file. OPTION4 applies to the bndout and elout files only. For the elout file OPTION4 is an integer variable that gives the number of additional history variables written into the elout file for each integration point in the beam elements. See Remark 7 below for the elout file and Remark 9 for the bndout file. OPTION1 OPTION2 OPTION3 OPTION4 The following Card 2 applies only to *DATABASE_NCFORC_FILTER Card 2 1 2 3 4 5 6 7 8 Variable RATE CUTOFF WINDOW TYPE Type F F F Default none none none I 0 0 0 0 0 VARIABLE DESCRIPTION RATE Time interval 𝑇 between filter sampling. CUTOFF Frequency cut-off 𝐶 in Hz. WINDOW The width of the window 𝑊 in units of time for storing the single, forward filtering required for the TYPE = 2 filter option. Increasing the width of the window will increase the memory required for the analysis. A window that is too narrow will reduce the amplitude of the filtered result significantly, and values below 15 are not recommended for that reason. In general, the results for the TYPE = 2 option are sensitive to the width of the window and experimentation is required. TYPE Flag for filtering options. EQ.0: No filtering (default). EQ.1: Single pass, forward Butterworth filtering. EQ.2: Two pass filtering over the specified time window. Backward Butterworth filtering is applied to the forward Butterworth results that have been stored. This option improves the phase accuracy significantly at the expense of memory. The file names and corresponding unit numbers are: Description I/O Unit # File Name Airbag statistics 43 Automatic tiebreak damage 92 ASCII database Boundary conditions 44 46 abstat atdout avsflt bndout (nodal forces and energies) Description I/O Unit # File Name Smug animator database Discrete elements 40 36 Discrete elements mass flow 219 Discrete beam elements 215 Element data Contact entities Global data Joint forces Material energies MOVIE file family MPGS file family Nastran/BDF file Nodal interface forces Nodal force group Nodal point data Pulley element data Pressure tube data Rigid body data Resultant interface forces Rigidwall forces Seat belts Cross-section forces Interface energies SPC reaction forces SPH element data Subsystems statistics Nodal constraint resultants Thermal output Tracer particles 34 48 35 53 37 50 50 49 38 45 33 216 421 47 39 32 52 31 51 41 68 58 42 73 70 defgeo deforc demflow disbout elout gceout glstat jntforc matsum moviennn.xxx where.nnn=001-999 mpgsnnn.xxx where nnn = 001-999 nasbdf ncforc nodfor nodout pllyout prtube rbdout rcforc rwforc sbtout secforc sleout spcforc sphout ssstat swforc (spot welds/rivets) tprint trhist Output Components for ASCII Files. ABSTAT BNDOUT DCFAIL x, y, z force energies moment (rigid bodies) volume pressure internal energy input mass flow rate output mass flow rate mass temperature density failure function normal term bending term shear term weld area effective strain rate axial force shear force torsional moment bending moment DEFORC x, y, z force ELOUT (t)Shells xx, yy, zz stress xy, yz, zx stress plastic strain xx, yy, zz strain† xy, yz, zx strain† Beams axial force resultant s shear resultant t shear resultant s moment resultant t moment resultant torsional resultant Solids xx, yy, zz stress xy, yz, zx stress effective stress yield function xx, yy, zz strain† xy, yz, zx strain† † Strains written for solids and for lower and upper integration points of shells and tshells if STRFLG = 1 in *DATABASE_EXTENT_BINARY. GCEOUT x, y, z force x, y, z moment time step kinetic energy internal energy sprint and damper energy hourglass energy system damping energy sliding interface energy eroded kinetic energy eroded internal energy eroded hourglass energy added mass GLSTAT total energy external work total and initial energy energy ratio without eroded energy element & part ID controlling time step global x, y, z velocity time per zone cycle joint internal energy stonewall energy rigid body stopper energy percentage [mass] increase JNTFORC x, y, z force x, y, z moment MATSUM kinetic energy internal energy hourglass energy x, y, z momentum x, y, z rigid body velocity eroded internal energy eroded kinetic energy added mass NCFORC NODOUT X force Y force Z force x, y, z displacement X, y, z velocity X, y, z acceleration X, y, z rotation X, y, z rotational velocity X, y, z rotation acceleration NODFOR X, y. z force PRTUBE cross section area pressure velocity density PLLYOUT RBDOUT RCFORC adjacent beam IDs slip slip rate resultant force wrap angle x, y, z displacement x, y, z velocity x, y, z acceleration x, y, z force Mass of nodes in contact RWFORC SECFORC SLEOUT normal x, y, z force x, y, z force x, y, z moment x, y, z center area resultant force slave energy master energy frictional energy SPCFORC SWFORC SPHOUT x, y, z force x, y, z moment axial force shear force failure function weld length resultant moment torsion xx, yy, zz stress xy, yz, zx stress density number of neighbors xx, yy, zz strain xy, yz, zx strain half of smoothing length plastic strain particle active state effective stress temperature xx,yy,zz strain rate xy,yz,zx strain rate SPH to SPH coupling forces Remarks: 1. Discrepancies Between “matsum” and “glstat” Output. The kinetic energy quantities in the matsum and glstat files may differ slightly in values for several reasons. First, the energy associated with added mass (from mass-scaling) is included in the glstat calculation, but is not included in matsum. Secondly, the energies are computed element by element in matsum for the deformable mate- rials and, consequently, nodes which are merged with rigid bodies will also have their kinetic energy included in the rigid body total. Furthermore, kinetic energy is computed from nodal velocities in glstat and from element midpoint velocities in matsum. 2. PRINT Keyword Option on *PART. The PRINT option in the part definition allows some control over the extent of the data that is written into the matsum and rbdout files. If the print option is used the variable PRBF can be defined such that the following numbers take on the meanings: EQ.0: default is taken from the keyword *CONTROL_OUTPUT, EQ.1: write data into rbdout file only, EQ.2: write data into matsum file only, EQ.3: do not write data into rbdout and matsum. Also see CONTROL_OUTPUT and PART_PRINT. 3. The Restart Feature. This keyword is also used in the restart phase, see *RESTART. Thus, the output interval can be changed when restarting. 4. LS-PrePost. All information in the files except in AVSFLT, MOVIE, and MPGS can also be plotted using LS-PrePost. Arbitrary cross plotting of results be- tween ASCII files is easily handled. 5. The “rcforc” File. Resultant contact forces reported in rcforc are averaged over the preceding output interval. 6. Spring and Damper Energy. “Spring and damper energy” reported in glstat is a subset of “Internal energy”. The “Spring and damper energy” includes internal energy of discrete elements, seatbelt elements, and that associated with joint stiffness. 7. OPTIONn Field for “elout”. OPTION1, OPTION2, OPTION3, and OPTION4 give the number of additional history variables output for the integrated solids, shells, thick shells, and beams, respectively. Within this special option, each integration point is printed with its corresponding history data. No integration points are averaged. This is different than the default output where the stress data within a shell ply of a fully integrated shell, for example, are averaged and then written as output. The primary purpose of this database extension is to allow the actual integration point stress data and history variable data to be checked. There are no transformations applied to either the output stresses or history data. 8. The Failure Function. The failure function reported to the DCFAIL database is set to zero when the weld fails. If damage is active, then it is set to the negative of the damage scale factor which goes from 1 to 0 as damage grows. 9. OPTIONn Field for “bndout”. For the bndout file, OPTION1 controls the nodal force group output, OPTION2 controls the concentrated force output, OPTION3 controls the pressure boundary condition output, and OPTION4 controls the velocity/displacement/acceleration nodal boundary conditions. If the value is 0 or left blank, the category is included (the default), and if it is 1, the category is not included in the bndout file. 10. Contents of “glstat”. The glstat table above includes all items that may appear in the glstat data. The items that are actually written depend on the contents of the input deck. For example, hourglass energy appears only if HGEN = 2 in *CONTROL_ENERGY and added mass only appears if DT2MS < 0 in *CON- TROL_TIMESTEP. 11. Element ID Controlling the Time Step. The element ID controlling the time step is included in the glstat data but is not read by LS-PrePost. If the element ID is of interest to the user, the ASCII version of the glstat file can be opened with a text editor. 12. The FILTER Option. The FILTER option uses a Butterworth filter for the forward, single pass filtering and the backward, double pass filtering options. The forward filtered output 𝑌(𝑛) at sampling interval 𝑛 is obtained from the solution value 𝑋(𝑛) using the formula 𝑌(𝑛) = 𝑎0𝑋(𝑛) + 𝑎1𝑋(𝑛 − 1) + 𝑎2𝑋(𝑛 − 2) + 𝑏1𝑌(𝑛 − 1) + 𝑏2𝑌(𝑛 − 2) where the coefficients are 𝜔𝑑 = 2𝜋 ( 0.6 ) 1.25 𝜔𝑎 = tan(𝜔𝑎 𝑇/2) 2/(1 + √2𝜔𝑎 + 𝜔𝑎 2) 𝑎0 = 𝜔𝑎 𝑎1 = 2𝑎0 𝑎2 = 𝑎0 𝑏1 = 2(1 − 𝜔𝑎 2)/(1 + √2𝜔𝑎 + 𝜔𝑎 2) 𝑏2 = (−1 + √2𝜔𝑎 − 𝜔𝑎 2)/(1 + √2𝜔𝑎 + 𝜔𝑎 2) The two previous solution values and filtered values at 𝑛 − 1 and 𝑛 − 2 are stored. Backward filtering improves the phase response of the filtered output. It is performed according to the formula 𝑍(𝑛) = 𝑎0𝑌(𝑛) + 𝑎1𝑌(𝑛 + 1) + 𝑎2𝑌(𝑛 + 2) + 𝑏1𝑍(𝑛 + 1) + 𝑏2𝑍(𝑛 + 2) where 𝑍(𝑛) is the backward filtered value at sample time 𝑛. This implies that all the forward filtered values 𝑌(𝑛) are stored during the analysis, and that would require a prohibitive amount of memory. To limit the amount of memory required, the forward filtered values at stored for the time interval 𝑊, where the number of stored states is 𝑊/𝑇, and the backward filtering is applied starting at the last saved value of the forward filtered values. As the window width increases, the filtered values approach the values that would be obtained from storing all of the forward filtered values. The results of the backward filtering are sensitive to the window width, and experimentation with the width is necessary to obtain good results with the minimum window width. A window width of at least 10 to 15 times the sam- ple rate 𝑇 should be used as a starting point. Some applications may require a window width that is much larger. The required window width decreases as the cut-off frequency increases. Or, to put it another way, the window width must be increased to make the filtered output smoother. As an example, a random series of numbers between 0 and 1 was generated and filtered at intervals of 0.1 milliseconds with cut-off frequencies from 60 Hz to 420 Hz. The reverse filtering was applied with various window widths to de- termine how many forward filtered states must be saved to achieve fixed levels of accuracy compared to complete reverse filtering from the last state to the first state. The results are shown in the table below. Note that the error is calculated only for the first state and the numbers being filtered are random. This example should only be used as a very rough guide that indicates the overall trends and not as a recommendation for specific problems. Cut-off Frequency No. of States 50% Error No. of States 25% Error No. of States 10% Error No. of States 5% Error No. of States 1% Error 60 Hz 120 Hz 180 Hz 240 Hz 300 Hz 360 Hz 420 Hz 26 13 8 6 5 5 4 33 16 10 8 6 6 5 55 30 22 17 12 10 9 68 37 26 19 15 12 10 87 44 30 23 18 16 15 *DATABASE Purpose: For each ALE group (or material), this card controls the output for element time-history variables (in a tabular format that can be plotted in LS-PrePost by using the XYPlot button). Card 1 1 2 3 4 5 6 7 8 Variable DTOUT SETID Type F I Default none none Variable Cards. Optional cards that can be used to add more variables with the volume fractions in the database (the volume fractions are always output). Include as many cards as necessary. This input ends at the next keyword (“*”) card. Card 2 1 2 3 4 5 6 7 8 Variable VAR VAR VAR VAR VAR VAR VAR VAR Type Default I 0 I 0 I 0 I 0 I 0 I 0 I 0 I 0 VARIABLE DESCRIPTION DTOUT Time interval between the outputs SETID ALE element set ID. If the model is 1D (*SECTION_ALE1D), the set should be *SET_BEAM If the model is 2D (*SECTION_ALE2D), the set should be *SET_SHELL If the model is 3D (*SECTION_SOLID), the set should be *SET_SOLID VARIABLE DESCRIPTION VAR Variable rank in the following list: EQ.1: xx-stress EQ.2: yy-stress EQ.3: zz-stress EQ.4: xy-stress EQ.5: yz-stress EQ.6: zx-stress EQ.7: plastic strain EQ.8: internal energy EQ.9: bulk viscosity EQ.10: previous volume EQ.11: pressure EQ.12: mass EQ.13: volume EQ.14: density EQ.15: kinetic energy If there is a blank column between 2 variable ranks, the list between these 2 ranks is selected. For example, if the card is as follows: 1, ,6 The 6 stresses are added to the database. Remarks: 1. The .xy files are created when the termination time is reached or if one of the following switches (after pressing the keys Ctrl - C) stops the job: sw1, stop, quit. During the run, they can be created with the switch sw2. 2. The .xy files are created by element. There is a curve by ALE group (or material). A last curve can be added for volume averaged variables. *DATABASE Purpose: For each ALE group (or material), this card activates extra output for: 1. material volume: alematvol.xy, 2. material mass: alematmas.xy, 3. internal energy: alematEint.xy, 4. kinetic energy: alematEkin.xy, 5. and kinetic energy loss during the advection: alematEkinlos.xy. These files are written in the “.xy” format, which LS-PrePost can plot with its “XYPlot” button. Card 1 2 3 4 5 6 7 8 Variable DTOUT BOXLOW BOXUP Type F Default none I 0 I 0 VARIABLE DESCRIPTION DTOUT Time interval between the outputs BOXLOW, BOXUP Range of *DEFINE_BOX ids. BOXLOW is the lower bound for the range while BOXUP is the upper bound. The series of volumes covered by the specified range of *DEFINE_BOX determines the mesh regions for which ALE material data are to be output. Remarks: The “.xy” files are created at termination or if one of the following switches (Ctrl-C) is encountered: sw2, sw1, stop, quit. *DATABASE_BINARY_OPTION1_OPTION2 keyword This *DATABASE_EXTENT_BINARY. used is to request binary output. See also Choices for OPTION1 are: BLSTFOR Blast pressure database. See also *LOAD_BLAST_ENHANCED and Remark 3. CPMFOR Corpuscular Particle Method interface force database. see Remark 2. D3DRLF Dynamic relaxation database. D3DUMP D3PART D3PLOT D3PROP D3THDT Database for restarts. Define output frequency in cycles. Database for subset of parts. See also *DATABASE_EXTENT_BI- NARY and *DATABASE_EXTENT_D3PART. Database for entire model. See also *DATABASE_EXTENT_BINA- RY. Database containing property data. See *DATABASE_BINARY_- D3PROP. Database containing time histories for subsets of elements and nodes. See *DATABASE_HISTORY. This database includes no ge- ometry. DEMFOR DEM interface force database. See Remark 5. FSIFOR FSILNK RUNRSF INTFOR ALE interface force database. See Remark 1. ALE interface linking database. See Remark 4. Database for restarts. Define output frequency in cycles. Contact interface database. Its file name must either be given using the FILE option or on the execution line using "S=". Also see *CONTACT variables SPR and MPR. PBMFOR Particle Blast Method interface force database. D3CRACK Option to control output interval for ASCII “aea_crack” file for the Winfrith concrete model (*MAT_084/085). Oddly, this command does not control the output of the binary crack database for the Win- frith concrete model. The binary crack database is written when “q=” appears on the execution line and its output interval is taken from *DATABASE_BINARY_D3PLOT, It is used by LS-PrePost to- gether with the D3PLOT database to display cracks in the deformed Winfrith concrete materials. OPTION2 only applies when OPTION1 is set to INTFOR and the only choice for OPTION2 is FILE. *DATABASE_BINARY_INTFOR_FILE requires one extra line of input that specifies the name of the intfor database. The D3DUMP and the RUNRSF options create complete databases which are necessary for restarts, see *RESTART. When RUNRSF is specified, the same file is overwritten after each interval, an option allows a series of files to be overwritten in a cyclic order. When D3DUMP is specified, a new restart file is created after each interva, thus a “family” of files is created numbered sequentially, e.g., d3dump01, d3dump02, etc. The default file names are runrsf and d3dump unless other names are specified on the execution line, see the INTRODUCTION, EXECUTION SYNTAX. Since all data held in memory is written into the restart files, these files can be quite large and care should be taken with the d3dump files not to create too many. If *DATABASE_BINARY_D3PLOT is not specified in the keyword deck then the output interval for d3plot is automatically set to 1/20th the termination time. The d3plot, d3part, d3drlf, and intfor databases contain histories of geometry and of state variables. Thus using these databases, one can, e.g., animate deformed geometry and plot time histories of element stresses and nodal displacements with LS-PrePost. The d3thdt database contains no geometry but rather time history data for element subsets as well as global information, see *DATABASE_HISTORY. This data can be plotted with LS-PrePost. The intfor database does not have a default filename and one must be specified by adding s=filename to the execution line. Similarly, for the fsifor database, a unique filename must be specified on the execution line with h=filename; see the INTRODUCTION, EXECUTION SYNTAX. The file structure is such that each file contains the full geometry at the beginning, followed by the analysis generated output data at the specified time intervals. For the contents of the d3plot, d3part and d3thdt databases, see also the *DATABASE_- EXTENT_BINARY definition. It is possible to restrict the information that is dumped and consequently reduce the size of the databases. The contents of the d3thdt database are also specified with the *DATABASE_HISTORY definition. It should also be noted in particular that the databases can be considerably reduced for models with rigid bodies containing many elements. FILE Card: Provide this card only for *DATABASE_BINARY_INTFOR_FILE. FILE Card 1 2 3 4 5 6 7 8 Variable Type Default VARIABLE FNAME FNAME A80 none DESCRIPTION Name of the database for the intfor data. S = filename on the execution line will override FNAME. Card 1 1 2 3 4 5 6 7 8 Variable DT/CYCL LCDT/NR BEAM NPLTC PSETID CID Type Default F - I - I - I - I - I - D3PLOT Card. Additional Card for D3PLOT option. Card 2 1 2 3 4 5 6 7 8 Variable IOOPT RATE CUTOFF WINDOW TYPE PSET Type Default I 0 F F F none none none I 0 I VARIABLE DT / CYL NR LCDT DESCRIPTION This field defines the time interval between output states, DT, for all options except D3DUMP, RUNRSF, and D3DRLF. For D3DUMP, RUNRSF, and D3DRLF options the first field contains CYCL instead of DT. These databases are updated every CYCL convergence checks during the explicit dynamic relaxation phase. Number of RUNning ReStart Files, runrsf, written in a cyclical fashion. The default is 1, i.e., only one runrsf file is created and the data therein is overwritten each time data is output. Optional load curve ID specifying time interval between dumps. This variable is only available for options D3PLOT, D3PART, D3THDT, INTFOR and BLSTFOR. VARIABLE BEAM NPLTC CID DESCRIPTION Discrete element option flag (*DATABASE_BINARY_D3PLOT only). EQ.0: Discrete spring and damper elements are added to the d3plot database where they are displayed as beam ele- ments. The discrete elements’ global 𝑥, global 𝑦, global 𝑧 and resultant forces (moments), and change in length (rotation) are written to the database where LS-PrePost (incorrectly) labels them as though they were beam quantities, i.e., axial force, S-shear resultant, T-shear re- sultant, etc. EQ.1: No discrete spring, damper and seatbelt elements are added to the d3plot database. This option is useful when translating old LS-DYNA input decks to KEYWORD input. In older input decks there is no requirement that beam and spring elements have unique ID's, and beam elements may be created for the spring and dampers with identical ID's to existing beam elements causing a fatal error. However, this option comes with some limi- tations and, therefore, should be used with caution. 1. Contact interfaces which are based on part IDs of seatbelt elements will not be properly gener- ated if this option is used. 2. DEFORMABLE_TO_RIGID will not work if PID refers to discrete, damper, or seatbelt elements. EQ.2: Discrete spring and damper elements are added to the d3plot database where they are displayed as beam ele- ments (similar to option 0). In this option the element resultant force is written to its first database position allowing beam axial forces and spring resultant forces to be plotted at the same time. This can be useful during some post-processing applications. This flag, set in *DATABASE_BINARY_D3PLOT, also affects the display of discrete elements in several other databases such as d3drlf, d3part. DT = ENDTIME/NPLTC. Applies to D3PLOT and D3PART options only. This overrides the DT specified in the first field. Coordinate system ID for FSIFOR and FSILNK, see *DEFINE_CO- ORDINATE_SYSTEM. VARIABLE PSETID DESCRIPTION Part set ID for D3PART and D3PLOT options only. See *SET_- PART. Parts in PSETID will excluded in the d3plot database. Onlyparts in PSETID are included in the d3part database. IOOPT This variable applies to the D3PLOT option only. Flag to govern behavior of the plot frequency load curve defined by LCDT: EQ.1: At the time each plot is generated, the load curve value is added to the current time to determine the next plot time (this is the default behavior). EQ.2: At the time each plot is generated, the next plot time T is computed so that T = the current time plus the load curve value at time T. EQ.3: A plot is generated for each abscissa point in the load curve definition. The actual value of the load curve is ignored. RATE Time interval 𝑇 between filter sampling. CUTOFF Frequency cut-off 𝐶 in Hz. WINDOW The width of the window 𝑊 in units of time for storing the single, forward filtering required for the TYPE = 2 filter option. Increasing the width of the window will increase the memory required for the analysis. A window that is too narrow will reduce the amplitude of the filtered result significantly, and values below 15 are not recommended for that reason. In general, the results for the TYPE = 2 option are sensitive to the width of the window and experimentation is required. TYPE Flag for filtering options. EQ.0: No filtering (default). EQ.1: Single pass, forward Butterworth filtering. EQ.2: Two pass filtering over the specified time window. Backward Butterworth filtering is applied to the forward Butterworth results that have been stored. This option improves the phase accuracy significantly at the expense of memory. PSET *DATABASE_BINARY DESCRIPTION Part set ID for filtering. If no set is specified, all parts are included. For each element integration point in the d3plot file, 24 words of memory are required in LS-DYNA for the single pass filtering, and more for the two pass filtering. Specifying PSET is recommended to minimize the memory requirements. Remarks: 1. FSIFOR. *DATABASE_BINARY_FSIFOR only applies to models having penalty-based coupling between Lagrangian and ALE materials (CTYPE=4 or 5 in the coupling card, *CONSTRAINED_LAGRANGE_IN_SOLID). When *DATABASE_FSI is defined, a few pieces of coupling information of some Lagrangian surface entities interacting with the ALE materials may be output as history parameters into a file called “dbfsi”. Coupling pressure is one of the output variables. However, this coupling pressure is averaged over the whole surface entity being monitored. To obtain coupling pressure contour plot as a function of time over the coupled surface, a user can define the *DATABASE_- BINARY_FSIFOR keyword. To use it, three things must be done: a) The INTFORC parameter (*CONSTRAINED_LAGRANGE_IN_SOLID, 4th row, 3rd column) must be turned ON (INTFORC = 1). b) A *DATABASE_BINARY_FSIFOR card is defined controlling the output interval. The time interval between output is defined by the parameter DT in this card. c) This interface force file is activated by executing LS-DYNA as follows: lsdyna i=inputfilename.k ... h=interfaceforcefilename LS-DYNA will then write out the segment coupling pressure and forces to a binary interface force file for contour plotting over the whole simula- tion interval. To plot the binary data in this file, type: lsprepost interfaceforcefilename. For example, when all 3 of the above actions are taken, and assuming “h” is set to “fsifor”, then a series of “fsifor##” binary files are output for contour plotting. To plot this, type “lsprepost fsifor” (without the dou- ble quotes). 2. CPMFOR. *DATABASE_BINARY_CPMFOR applies to models using *AIRBAG_PARTICLE feature which controls the output interval of CPM inter- face force file. This interface force file is activated by executing LS-DYNA with command line option (cpm=). lsdyna i=inputfilename.k … cpm=interfaceforce_filename CPM interface force file stores segment’s coupling pressure and forces. The coupling pressure is averaged over each segment without considering the effect of ambient pressure, 𝑃atm. 3. BLSTFOR. The BLSTFOR database is not available for two dimensional axisymmetric analysis. 4. FSILNK. The *DATABASE_BINARY_FSILNK variant writes the selected *CONSTRAINED_LAGRANGE_IN_SOLID interface’s segment pressure to the fsilink file for the next analysis without ALE meshes. lsdyna i=inputfilename.k … fsilink=filename 5. DEMFOR. *DATABASE_BINARY_DEMFOR applies to models using DEM coupling option *DEFINE_DE_TO_SURFACE_COUPLING. This card will control the output interval of DEM interface force file. This interface force file is activated by LS-DYNA command line option (dem=). lsdyna i=inputfilename.k … dem=interfaceforce_filename DEM interface force file stores segment’s coupling pressure and forces. 6. PBMFOR. *DATABASE_BINARY_PBMFOR applies to models using *PARTI- CLE_BLAST feature which controls the output interval of PBM interface force file. This interface force file is activated by executing LS-DYNA with command line option (pbm=). lsdyna i=inputfilename.k … pbm=interfaceforce_filename PBM interface force file stores segment’s coupling pressure and forces. *DATABASE_BINARY Purpose: This card causes LS-DYNA to add the part, material, equation of state, section, and hourglass data to the first d3plot file or else write the data to a separate database d3prop. Rigidwall data can also be included. LS-PrePost does not read the additional data so use of this command is of dubious benefit. Card 1 1 2 3 4 5 6 7 8 Variable IFILE IMATL IWALL Type Default I 1 I 0 I 0 VARIABLE IFILE DESCRIPTION Specify file for d3prop output. (This can also be defined on the command line by adding d3prop = 1 or d3prop = 2 which also sets IMATL = IWALL = 1) EQ.1: Output data at the end of the first d3plot file. EQ.2: Output data to the file d3prop. IMATL Output *EOS, *HOURGLASS, *MAT, *PART and *SECTION data. EQ.0: No EQ.1: Yes IWALL Output *RIGIDWALL data. EQ.0: No EQ.1: Yes . *DATABASE Purpose: This card activates an ASCII file “cpm_sensor”. Its input defines sensors’ locations based on the positions of some Lagrangian segments. The output gives the history of the velocity, temperature, density and pressure averaged on the number of particles contained in the sensors. This card is activated only when the *AIRBAG_PAR- TICLE card is used. Card 1 1 2 3 4 5 6 7 8 Variable DT BINARY Type F I Sensor Definition Cards. Each card defines one sensor. This card may be repeated to define multiple sensors. Input stops when the next “*” Keyword is found. 6 7 8 Card 2 1 2 3 4 Variable SEGID OFFSET R/LX LEN/LY Type I F F F 5 LZ F VARIABLE DESCRIPTION DT Output interval BINARY Flag for the binary file EQ.1: ASCII file is written, EQ.2: Data written to the binary file “binout”, EQ.3: ASCII file is written and the data written to the binary file “binout”. SEGID Segment set ID OFFSET Offset distance between the center of the sphere sensor and the segment center. If it is positive, Or, the distance between the base of the cylinder and the segment center while LENGTH is not zero. it is on the side pointed to by the segment normal vector. See remarks1 and 3. R/LX *DATABASE_CPM_SENSOR DESCRIPTION Radius(sphere)/length in local X direction(rectangular) of the sensor. See remarks 2 and 3. LEN/LY Length(cylinder)/length in local Y direction(rectangular) of the sensor. LZ Length in local Z direction(rectangular) of the sensor see remark 4 Remarks: 1. Each segment has a sensor. The distance between the segment center and the sensor center is defined by OFFSET (2nd parameter on the 2nd line) in the normal direction defined by the segment. This distance is constant: the sensor moves along with the segment. 2. The sensor is a sphere with a radius given by RADIUS (3rd parameter on the 2nd line). 3. OFFSET should be larger than RADIUS to prevent the segment from cutting the sphere. For cylindrical sensor, OFFSET is the distance from segment to the base of the cylinder. 4. For rectangular sensor, OFFSET is the distance from reference segment to the sensor. The sensor is defined using the segment’s coordinates system. The base point is n1 and local X direction is along the vector n2 - n1. The local Z direc- tion is the segment normal direction and local Y direction is constructed by local X and Z directions. 5. The output parameters in the “cpm_sensor” file are: velx vely velz velr temp dens pres = x-velocity = y-velocity = z-velocity = velocity = = density = pressure temperature These values are averaged on the number of particles in the sensor. RADIUS should be large enough to contain a reasonable number of particles for the averages. $...|....1....|....2....|....3....|....4....|....5....|....6....|....7....|. $ INPUT: $...|....1....|....2....|....3....|....4....|....5....|....6....|....7....|. *DATABASE_CPM_SENSOR 0.01 $ SEGSID OFFSET RADIUS LENGTH 123 5.0 5.0 124 -0.2 0.1 125 0.7 0.6 1.0 $...|....1....|....2....|....3....|....4....|....5....|....6....|....7....|.. $ The segment set id: 123 has 1 segment. $ The segment set id: 123 has 1 segment. $ The segment set id: 123 has 11 segments. $ Each segment has an ID defined in D3HSP $ The D3HSP file looks like the following: $...|....1....|....2....|....3....|....4....|....5....|....6....|....7....|.. Segments for sensor 1 Sensor id n1 n2 n3 n4 1 3842 3843 3848 3847 Segments for sensor 2 Sensor id n1 n2 n3 n4 2 3947 3948 3953 3952 Segments for sensor 3 Sensor id n1 n2 n3 n4 3 3867 3868 2146 2145 4 3862 3863 3868 3867 5 3857 3858 3863 3862 6 3852 3853 3858 3857 7 3847 3848 3853 3852 8 3837 3838 3843 3842 9 3842 3843 3848 3847 10 3832 3833 3838 3837 11 3827 3828 3833 3832 12 3822 3823 3828 3827 13 1125 1126 3823 3822 $...|....1....|....2....|....3....|....4....|....5....|....6....|....7....|.. *DATABASE_CROSS_SECTION_OPTION1_{OPTION2} Option 1 includes: PLANE SET To define an ID and heading for the database cross section use the option: ID Purpose: Define a cross section for resultant forces written to ASCII file secforc. 1. For the PLANE option, a set of two cards is required for each cross section. Then a cutting plane has to be defined, see Figure 14-1. 2. If the SET option is used, just one card is needed which identifies a node set and at least one element set. In this case the node set(s) defines the cross section, and the forces from the elements belonging to the element set(s) are summed up to calculate the section forces. Thus the element set(s) should include ele- ments on only one side (not both sides) of the cross section. The cross-section should cut through deformable elements only, not rigid bodies. Cutting through master segments for deformable solid element spot welds can lead to incorrect section forces since the constraint forces are not accounted for in the force and moment summations. Beam element modeling of welds do not require any special precautions. ID Card. Additional card for ID keyword option. Optional 1 2 3 4 5 6 7 8 Variable CSID Type I HEADING A70 The heading is picked up by some of the peripheral LS-DYNA codes to aid in post- processing. VARIABLE DESCRIPTION CSID Cross section ID. This must be a unique number. HEADING Cross section descriptor. It is suggested that unique descriptions be used. Plane Card 1. First additional card for PLANE keyword option. Card 1 1 2 3 4 5 6 7 8 Variable PSID XCT YCT ZCT XCH YCH ZCH RADIUS Type Default I 0 F 0. F 0. F 0. F 0. F 0. F 0. F 0. Plane Card 2. Second additional card for PLANE keyword option. Card 2 1 2 3 4 5 Variable XHEV YHEV ZHEV LENL LENM Type F Default 0. F 0. F F F 0. infinity infinity global 6 ID I 7 8 ITYPE I 0 The set option requires that the equivalent of the automatically generated input by the cutting plane capability be identified manually and defined in sets. All nodes in the cross-section and their related elements that contribute to the cross-sectional force resultants must be defined. Set Card. Additional Card for the SET keyword option. Card 1 1 2 3 4 5 6 Variable NSID HSID BSID SSID TSID DSID Type I I Default required 0 I 0 I 0 I 0 I 0 7 ID I global 8 ITYPE I *DATABASE_CROSS_SECTION Resultants are computed on this plane Origin of cutting plane Figure 14-1. Definition of cutting plane for automatic definition of interface for cross-sectional forces. The automatic definition does not check for springs and dampers in the section. For best results the cutting plane should cleanly pass through the middle of the elements, distributing them equally on either side. Elements that intersect the edges of the cutting plane are deleted from the the cross-section. VARIABLE DESCRIPTION CSID PSID XCT YCT ZCT XCH Optional ID for cross section. If not specified cross section ID is taken to be the cross section order in the input deck. Part set ID. If zero all parts are included. 𝑥-coordinate of tail of any outward drawn normal vector, N, originating on wall (tail) and terminating in space (head), see Figure 14-1. 𝑦-coordinate of tail of normal vector, 𝐍. 𝑧-coordinate of tail of normal vector, 𝐍. 𝑥-coordinate of head of normal vector, 𝐍. VARIABLE DESCRIPTION YCH ZCH RADIUS 𝑦-coordinate of head of normal vector, 𝐍. 𝑧-coordinate of head of normal vector, 𝐍. Optional radius. If a radius is set (radius ≠ 0), then circular cut plane centered at (XCT, YCT ,ZCT) of radius = RADIUS, with the normal vector originating at (XCT, YCT, ZCT) and pointing towards (XCH, YCH, ZCH) will be created. In this case the variables XHEV, YHEV, ZHEV, LENL, and LENM, which are defined on the 2nd card will be ignored. XHEV YHEV ZHEV LENL 𝑥-coordinate of head of edge vector, 𝐋. 𝑦-coordinate of head of edge vector, 𝐋. 𝑧-coordinate of head of edge vector, 𝐋. Length of edge 𝑎, in 𝐋 direction. LENM Length of edge 𝑏, in 𝐌 direction. NSID HSID BSID SSID TSID DSID ID Nodal set ID, see *SET_NODE_OPTION. Solid element set ID, see *SET_SOLID. Beam element set ID, see *SET_BEAM. Shell element set ID, see *SET_SHELL_OPTION. Thick shell element set ID, see *SET_TSHELL. Discrete element set ID, see *SET_DISCRETE. Rigid body , accelerometer ID , or coordinate ID, see *DEFINE_COORDINATE_NODES. The force resultants are output in the updated local system of the rigid body or accelerometer. For ITYPE = 2, the force resultants are output in the updated local coordinate system if FLAG = 1 in *DEFINE_CO- ORDINATE_NODES or if NID is nonzero in *DEFINE_COORDI- NATE_VECTOR. ITYPE *DATABASE_CROSS_SECTION DESCRIPTION Flag that specifies whether ID above pertains to a rigid body, an accelerometer, or a coordinate system. EQ.0: rigid body, EQ.1: accelerometer, EQ.2: coordinate system. Available options include: *DATABASE AVS BINARY D3PART INTFOR MOVIE MPGS SSSTAT Purpose: Control to some extent the content of specific output databases. The BINARY option of *DATABASE_EXTENT applies to the binary databases d3plot, d3thdt, and d3part. In the case of the d3part database, variables set using the D3PART option will override the corresponding variables of the BINARY option. See also *DATABASE_BINARY_OPTION. The AVS, MOVIE, and MPGS databases will be familiar to users that have a use for those databases. *DATABASE_EXTENT_AVS This command controls content written to the avsflt database. See AVSFLT option to *DATABASE card. Varriable Cards. Define as many cards as needed. Input ends at next keyword (“*”) card. Card 1 1 2 3 4 5 6 7 8 Variable VTYPE COMP Type I I VARIABLE DESCRIPTION VTYPE Variable type: EQ.0: node, EQ.1: brick, EQ.2: beam, EQ.3: shell, EQ.4: thick shell. Component components from the following tables can be chosen: the corresponding VTYPE, For ID. integer VTYPE.EQ.0: Table 10.1, VTYPE.EQ.1: Table 10.2, VTYPE.EQ.2: not supported, VTYPE.EQ.3: Table 10.3, VTYPE.EQ.4: not supported. COMP Remarks: The AVS database consists of a title card, then a control card defining the number of nodes, brick-like elements, beam elements, shell elements, and the number of nodal vectors, NV, written for each output interval. The next NV lines consist of character strings that describe the nodal vectors. Nodal coordinates and element connectivity follow. For each state the solution time is written, followed by the data requested below. The last word in the file is the number of states. We recommend creating this file and examining its contents, since the organization is relatively transparent. Table 14-2. Nodal Quantities Component ID Quantity 1 2 3 x, y, z-displacements x, y, z-velocities x, y, z-accelerations Table 14-3. Brick Element Quantities Component ID 1 2 3 4 5 6 7 Quantity x-stress y-stress z-stress xy-stress yz-stress zx-stress effective plastic strain Table 14-4. Shell and Thick Shell Element Quantities Component ID Quantity 1 2 3 4 5 6 7 8 9 10 11 12 13 14 15 16 17 18 19 20 21 22 23 24 25 26 27 28 29 midsurface x-stress midsurface y-stress midsurface z-stress midsurface xy-stress midsurface yz-stress midsurface xz-stress midsurface effective plastic strain inner surface x-stress inner surface y-stress inner surface z-stress inner surface xy-stress inner surface yz-stress inner surface zx-stress inner surface effective plastic strain outer surface x-stress outer surface y-stress outer surface z-stress outer surface xy-stress outer surface yz-stress outer surface zx-stress outer surface effective plastic strain bending moment-mxx (4-node shell) bending moment-myy (4-node shell) bending moment-mxy (4-node shell) shear resultant-qxx (4-node shell) shear resultant-qyy (4-node shell) normal resultant-nxx (4-node shell) normal resultant-nxx (4-node shell) normal resultant-nxx (4-node shell) Component ID Quantity 30 31 32 33 34 35 36 37 38 39 40 41 42 43 44 45 46 47 48 49 50 51 52 53 54 55 56 57 58 59 thickness (4-node shell) element dependent variable element dependent variable inner surface x-strain inner surface y-strain inner surface z-strain inner surface xy-strain inner surface yz-strain inner surface zx-strain outer surface x-strain outer surface y-strain outer surface z-strain outer surface xy-strain outer surface yz-strain outer surface zx-strain internal energy midsurface effective stress inner surface effective stress outer surface effective stress midsurface max. principal strain through thickness strain midsurface min. principal strain lower surface effective strain lower surface max. principal strain through thickness strain lower surface min. principal strain lower surface effective strain upper surface max. principal strain through thickness strain upper surface min. principal strain Component ID Quantity 60 upper surface effective strain Table 14-5. Beam Element Quantities Component ID Quantity 1 2 3 4 5 6 x-force resultant y-force resultant z-force resultant x-moment resultant y-moment resultant z-moment resultant *DATABASE_EXTENT_BINARY_{OPTION} Purpose: Control to some extent the content of binary output databases d3plot, d3thdt, and d3part. See also *DATABASE_BINARY_OPTION and *DATBASE_EXTENT_D3- PART. The content of the binary output database intfor may be modified using *DATA- BASE_EXTENT_INTFOR. The option COMP controls to the content of binary output databases d3plot and d3eigv. When the option COMP is used, it will suppress most of settings in *DATABASE_EXTENT_BINARY. Available options include: <BLANK> COMP If no option is specified, use the following cards: Card 1 1 2 3 4 5 6 7 8 Variable NEIPH NEIPS MAXINT STRFLG SIGFLG EPSFLG RLTFLG ENGFLG Type Default I 0 I 0 Remarks Card 2 1 2 I 3 1 3 I 1 I 1 I 1 I 1 I 0 10 4 5 6 7 8 Variable CMPFLG IEVERP BEAMIP DCOMP SHGE STSSZ N3THDT IALEMAT Type Default I 0 I 0 Remarks I 0 2 I 1 I 1 I 1 I 2 I *DATABASE_EXTENT_BINARY Card 3 1 2 3 4 5 6 7 8 Variable NINTSLD PKP_SEN SCLP HYDRO MSSCL THERM INTOUT NODOUT Type Default I 1 I 0 F 1.0 I 0 I 0 I 0 A A none none Remarks Card 4 1 2 3 4 5 6 4 7 4 8 Variable DTDT RESPLT NEIPB Type Default I 1 I 0 I 0 For COMP option, use Card 1 below (no Cards 2-4) Card 1 1 2 3 4 5 6 7 8 Variable IGLB IXYZ IVEL IACC ISTRS ISTRA ISED Type Default I 0 I 0 I 0 I 0 I 0 I 0 I 0 Remarks VARIABLE NEIPH NEIPS DESCRIPTION Number of additional integration point history variables written to the binary databases (d3plot, d3part, d3drlf) for solid elements and SPH particles. The integration point data is written in the same order that it is stored in memory-each material model has its own history variables that are stored. For user defined materials it is important to store the history data that is needed for plotting before the data which is not of interest. See also *DEFINE_MATE- RIAL_HISTORIES. For output of additional integration point history variables for solid elements to the elout database, see the variable OPTION1 in *DATABASE_ELOUT. Number of additional integration point history variables written to the binary databases (d3plot, d3part, d3drlf) for both shell and thick shell elements for each integration point, see NEIPH above and *DEFINE_MATERIAL_HISTORIES. For output of additional integration point history variables for shell and thick shell elements to the elout database, see the variables OPTION2 and OPTION3, respectively, in *DATABASE_ELOUT. VARIABLE MAXINT DESCRIPTION Number of shell and thick shell through-thickness integration points for which output is written to d3plot. This does not apply to strain tensor output flagged by STRFLG. MAXINT (def = 3) number of Integration Points Description > 3 (even & odd) results are output for the outermost (top) (bottom) and integration points together with results for the neutral axis. innermost 1 All three results are identical. 3 3 > 3 ≤ MAXINT ≠ 3 Even < 0 Any for the Results first MAXINT integration points in the element will be output. See above. This will exclude mid- results, whereas when surface MAXINT = 3 mid-surface results are calculated and reported. integration points are MAXINT output for each in plane integration point location and no averaging is used. This can greatly increase the size of the binary databases d3plot, d3thdt, and d3part. See Remark 1 for more information. VARIABLE DESCRIPTION STRFLG STRFLG is interpreted digit-wise STRFLG = [𝑁𝑀𝐿], STRFLG = 𝐿 + 𝑀 × 10 + 𝑁 × 100 L.EQ.1: Write strain tensor data to d3plot and elout. For shell and thick shell elements two tensors are written, one at the innermost and one at the outermost integration point. For solid elements a single strain tensor is writ- ten. M.EQ.1: Write plastic strain data to d3plot. N.EQ.1: Write thermal strain data to d3plot. Examples. For STRFLG = 11 (011) LS-DYNA will write both strain and plastic strain tensors, but no thermal strain tensors. Whereas for STRFLG = 110, LS-DYNA will write plastic and thermal strain tensors but no strain tensors. For more information and supported elements and materials, see Remark 10. SIGFLG Flag for including the stress tensor for shells and solids. EQ.1: include (default), EQ.2: exclude for shells, include for solids. EQ.3: exclude for shells and solids. EPSFLG Flag for including the effective plastic strains for shells and solids. EQ.1: include (default), EQ.2: exclude for shells, include for solids. EQ.3: exclude for shells and solids. RLTFLG Flag for including stress resultants in the shell LS-DYNA database: EQ.1: include (default), EQ.2: exclude. ENGFLG Flag for including shell internal energy density and shell thickness. EQ.1: include (default), EQ.2: exclude. CMPFLG *DATABASE_EXTENT_BINARY DESCRIPTION Flag to indicate the coordinate system for output of stress and strain in solids, shells and thick shells comprised of orthotropic or anisotropic materials. See Remark 4. EQ.-1: Same as 1, but for *MAT_FABRIC (forms 14 and -14) and *MAT_FABRIC_MAP the stress and strain is in engineer- ing quantities instead of Green-Lagrange strain and 2nd Piola-Kirchhoff stress. EQ.0: global coordinate system with exception of elout for shells . EQ.1: local material coordinate system (as defined by AOPT and associated parameters in the *MAT input, and if ap- plicable, by angles B1, B2, etc. in *SECTION_SHELL, *SECTION_TSHELL, or *PART_COMPOSITE, and by optional input in the *ELEMENT data). CMPFLG = 1 affects both d3plot and elout databases. IEVERP Every output state for the d3plot database is written to a separate file. EQ.0: more than one state can be on each plot file, EQ.1: one state only on each plot file. BEAMIP Number of beam integration points for output. This option does not apply to beams that use a resultant formulation. See Remark 2. VARIABLE DESCRIPTION DCOMP Data compression to eliminate rigid body data: EQ.1: off (default), no rigid body data compression, EQ.2: on, rigid body data compression active, EQ.3: off, no rigid body data compression, but all nodal velocities and accelerations are eliminated from the data- base. EQ.4: on, rigid body data compression active and all nodal velocities and accelerations are eliminated from the data- base. EQ.5: on, rigid body data compression active and rigid nodal data are eliminated from the database. Only 6 DOF rigid body motion is written. EQ.6: on, rigid body data compression active, rigid nodal data, and all nodal velocities and accelerations are eliminated from the database. Only 6 DOF rigid body motion is writ- ten. SHGE Flag for including shell hourglass energy density. EQ.1: off (default), no hourglass energy written, EQ.2: on. STSSZ Flag for including shell element time step, mass, or added mass. EQ.1: off (default), EQ.2: output time step size, EQ.3: output mass, added mass, or time step size. See Remark 3 below. N3THDT Flag for including material energy in d3thdt database. EQ.1: off, energy is NOT written to d3thdt database, EQ.2: on (default), energy is written to d3thdt database. IALEMAT Output solid part ID list containing ALE materials. EQ.1: on (default) NINTSLD PKP_SEN SCLP HYDRO *DATABASE_EXTENT_BINARY DESCRIPTION Number of solid element integration points written to the LS- DYNA database. When NINTSLD is set to 1 (default) or to any value other than 8, integration point values are averaged and only those averages are written output. To obtain values for individual integration points, set NINTSLD to 8, even if the multi-integration point solid has fewer than 8 integration points. Flag to output the peak pressure and surface energy computed by each contact interface into the interface force database. To obtain the surface energy, FRCENG, must be sent to 1 on the control contact card. When PKP_SEN = 1, it is possible to identify the energies generated on the upper and lower shell surfaces, which is important in metal forming applications. This data is mapped after each H-adaptive remeshing. EQ.0: No data is written EQ.1: Output the peak pressures and surface energy by contact interface A scaling parameter used in the computation of the peak pressure. This parameter is generally set to unity (the default), but it must be greater than 0. Either 3, 5 or 7 additional history variables useful to shock physics are output as the last history variables to d3plot (does not apply to elout). For HYDRO = 1, the internal energy per reference volume, the reference volume, and the pressure from bulk viscosity are added to the database, and for HYDRO = 2, the relative volume and current density are also added. For HYDRO = 4, two further variables are added: volumetric strain (defined as relative volume – 1.0), and Hourglass energy per unit initial volume. MSSCL Output nodal information related to mass scaling into the d3plot database. This option can be activated if and only if DT2MS < 0.0, see control card *CONTROL_TIMESTEP. EQ.0: No data is written EQ.1: Output incremental nodal mass EQ.2: Output percentage increase in nodal mass See Remark 3. VARIABLE THERM DESCRIPTION Output of thermal data to d3plot. The use of this option (THERM > 0) may make the database incompatible with other 3rd party software. EQ.0: (default) output temperature EQ.1: output temperature EQ.2: output temperature and flux EQ.3: output temperature, flux, and shell bottom and top surface temperature INTOUT Output stress/strain at all integration points for detailed element output in the ASCII file eloutdet. DT and BINARY of *DATA- BASE_ELOUT apply to eloutdet. See Remark 4. EQ.STRESS: when stress output is required EQ.STRAIN: when strain output is required EQ.ALL: when both stress and strain output are required NODOUT Output extrapolated stress/strain at connectivity nodes for detailed element output in the ASCII file eloutdet. DT and BINA- RY of *DATABASE_ELOUT apply to eloutdet. See Remark 4. EQ.STRESS: when stress output is required EQ.STRAIN: when strain output is required EQ.ALL: when both stress and strain output are required EQ.STRESS_GL: when nodal averaged stress output along the global coordinate system is required EQ.STRAIN_GL: when nodal averaged strain output along the global coordinate system is required EQ.ALL_GL: for global nodal averaged stress and strain output DTDT Output of node point Δtemperature/Δtime data to d3plot. EQ.0: (default) no output EQ.1: output Δ𝑇/Δ𝑡 RESPLT *DATABASE_EXTENT_BINARY DESCRIPTION Output of translational and rotational residual forces to d3plot and d3iter. EQ.0: No output EQ.1: Output residual NEIPB Number of additional element or integration point history variables written to the binary databases (d3plot, d3part, d3drlf) for beam elements, see NEIPH above, BEAMIP and *DEFINE_MA- TERIAL_HISTORIES. For output of additional integration point history variables for beam elements to the elout database, see the variable OPTION4 in *DATABASE_- ELOUT. See also Remark 12. IGLB Output flag for global data EQ.0: no EQ.1: yes IXYZ Output flag for geometry data EQ.0: no EQ.1: yes IVEL Output flag for velocity data EQ.0: no EQ.1: yes IACC Output flag for acceleration data EQ.0: no EQ.1: yes ISTRS Output flag for stress data EQ.0: no EQ.1: yes ISTRA Output flag for strain data EQ.0: no EQ.1: yes ISED Output flag for strain energy density data EQ.0: no EQ.1: yes Remarks: 1. MAXINT Field. If MAXINT is set to 3 then mid-surface, inner-surface and outer-surface stresses are output at the center of the element. For an even num- ber of integration points, the points closest to the center are averaged to obtain the midsurface values. If multiple integration points are used in the shell plane, the stresses at the center of the element are found by computing the average of these points. For MAXINT equal to 3, LS-DYNA assumes that the data for the user defined integration rules are ordered from bottom to top even if this is not the case. If MAXINT is not equal to 3, then the stresses at the center of the ele- ment are output in the order that they are stored for the selected integration rule. If multiple points are used in plane the stresses are first averaged. 2. BEAMIP Field. Beam stresses are output if and only if BEAMIP is greater than zero. In this latter case the data that is output is written in the same order that the integration points are defined. The data at each integration point consists of the following five values for elastic-plastic Hughes-Liu beams: the normal stress, 𝜎𝑟𝑟; the transverse shear stresses, σrs and σtr; the effective plastic strain, and the axial strain which is logarithmic. For beams that are not elastic-plastic, the first history variable, if any, is output instead of the plastic strain. For the beam elements of Belytschko and his co-workers, the transverse shear stress components are not used in the formulation. No data is output for the Be- lytschko-Schwer resultant beam. 3. Mass Scaling. If mass scaling is active, the output of the time step size reveals little information about the calculation. If global mass scaling is used for a constant time step, the total element mass is output; however, if the mass is increased so that a minimum time step size is maintained (DT2MS is negative), the added mass is output. Also, see the control card *CONTROL_TIMESTEP. 4. Output Coordinate System. Output coordinate system used. When the parameters: INTOUT or NODOUT is set to STRESS, STRAIN, or ALL, the out- put coordinate system of the data, similar to the ASCII file elout, is determined by CMPFLG in *DATABASE_EXTENT_BINARY. a) When NODOUT is set to STRESS, STRAIN , or ALL. Each node of the el- ement nodal connectivity will be output. See Example 1. b) Nodal output when NODOUT is set to STRESS_GL, STRAIN_GL, or ALL_GL. Averaged nodal results are calculated by summing up all con- tributions from elements sharing the common node, and then dividing the total by the number of contributing elements. Averaged nodal values are always output in the global coordinate system. See Example 2. 5. Contents of eloutdet. Available stress/strain components in eloutdet stress components includes 6 stress components (sig-𝑥𝑥, sig-𝑦𝑦, sig-𝑧𝑧, sig-𝑥𝑦, sig-𝑦𝑧, sig-𝑧𝑥), yielding status, and effective plastic strain. Strain components includes 6 strain components 6. Shell Element Output at Integration Points. stresses at all integration points can be output. The strain at the top and bottom integration layer can be output. At a connective node the extrapolated stress and strain at the top and bottom layer can be output 7. Thick Shells. Thick shell element output includes the six stress components at each integration point. Strain at the top and bottom layer can be output. At the element node, values at the bottom layer are extrapolated to yield the values of nodes 1-4, and values at the top layer are extrapolated to yield values of nodes 5-8. 8. Integration Point Locations. Stresses and strain at all integration points can be output. The integration point order is as follows: a) point #1 is the point closest to node #1 in the connectivity array b) point #2 is the closest point to node #2, etc c) For tetrahedrons type 4, 16 and 17 with 5 integration points, point #5 is the midpoint. d) For the nodal points, values at the integration points are extrapolated. 9. Reporting Residual Forces and Moments. The output of residual forces and moments is supported for implicit and double precision only. With this option the forces and moments appear under the Ndv button in the fringe menu in LS- PrePost. The residual for rigid bodies is distributed to the slave nodes for the body without scaling for the purpose of capturing the complete residual vector. 10. Calculation of Strains (STRFLG). The strain tensor 𝜺 that are output to the d3plot database are calculated using proper time integration of the rate-of- deformation tensor 𝐃. More specifically, to assert objectivity of the resulting strain, it is for solids using a Jaumann rate of strain whereas for shells it uses the co-rotational strain rate. In mathematical terms the integration is using the following strain rates 𝛆̇ = 𝐃 − 𝛆𝐖 + 𝐖𝛆 (solids) 𝛆̇ = 𝐃 − 𝛆𝛀 + 𝛀𝛆 (shells) where 𝐖 is the spin tensor and 𝛀 = 𝐐̇ 𝐐T is the rotational velocity of the co- rotational system 𝐐 used for the shell element in question, taking into account invariant node numbering and such. This is to say that the resulting strains would be equal to the Cauchy stress for a hypo-elastic material (MAT_ELAS- TIC) with a Young’s modulus of 1 and a Poisson’s ratio of 0. This should be kept in mind when interpreting the results since they are not invariant to changes in element formulations and possibly nodal connectivities. 11. Plastic and Thermal Strain (STRFLG). The algorithm for writing plastic and thermal strains, which is also activated using STRFLG, is a modification of the algorithm used for mechanical strains . a) For solids the element average strain in the global system having 6 com- ponents is written (local system if CMPFLG is set). b) For shells both plastic and thermal strains have 6 components. The ther- mal strain is written as a single tensor as in the solid case. The plastic strain output consists of 3 plane-averaged tensors: one for the bottom, one for the middle, and one for the top. For an even number of through thick- ness integration points, the middle is taken to be the average of the two in- tegration points closest to the mid surface. Currently, only the following element/materials combinations are supported but other will be added upon request. Thermal strain tensors Plastic strain tensors Shells Solids Materials Shells Solids Materials 2, 16, 23 1, 2 Add thermal expansion, 255 2, 16, 23 1, 2 24, 255 12. History Variables for Beams (NEIPB). In general, NEIPB follows the same conventions as NEIPH and NEIPS do for solid and shell elements and is sup- ported in LS-PrePost v4.3 or later. Average, min and max values for each ele- ment are output, including data for resultant elements. If BEAMIP is nonzero, then element data is complemented with BEAMIP integration point values that can be examined individually. Beam history data is post-processed similarly to that of solid and shell element history data. Example 1: Excerpt from eloutdet file for a shell element with two through-thickness integration points and four in-plane integration points, with INTOUT = STRESS and NO- DOUT = STRESS: element materl ipt stress sig-xx sig-yy sig-zz sig-xy sig0yz sig-zx yield location 1- 1 1- 10 elastic 4.41E-2 2.51E-1 0.00E+0 7.76E-8 0.00E+0 0.00E+0 0.00E+0 int. point 1 1- 10 elastic 4.41E-2 2.51E-1 0.00E+0 7.76E-8 0.00E+0 0.00E+0 0.00E+0 int. point 2 1- 10 elastic 4.41E-2 2.51E-1 0.00E+0 7.76E-8 0.00E+0 0.00E+0 0.00E+0 int. point 3 1- 10 elastic 4.41E-2 2.51E-1 0.00E+0 7.76E-8 0.00E+0 0.00E+0 0.00E+0 int. point 4 1- 10 elastic 4.41E-2 2.51E-1 0.00E+0 7.76E-8 0.00E+0 0.00E+0 0.00E+0 node 21 1- 10 elastic 4.41E-2 2.51E-1 0.00E+0 7.76E-8 0.00E+0 0.00E+0 0.00E+0 node 22 1- 10 elastic 4.41E-2 2.51E-1 0.00E+0 7.76E-8 0.00E+0 0.00E+0 0.00E+0 node 20 1- 10 elastic 4.41E-2 2.51E-1 0.00E+0 7.76E-8 0.00E+0 0.00E+0 0.00E+0 node 19 2- 10 elastic 4.41E-2 2.51E-1 0.00E+0 7.76E-8 0.00E+0 0.00E+0 0.00E+0 int. point 1 2- 10 elastic 4.41E-2 2.51E-1 0.00E+0 7.76E-8 0.00E+0 0.00E+0 0.00E+0 int. point 2 2- 10 elastic 4.41E-2 2.51E-1 0.00E+0 7.76E-8 0.00E+0 0.00E+0 0.00E+0 int. point 3 2- 10 elastic 4.41E-2 2.51E-1 0.00E+0 7.76E-8 0.00E+0 0.00E+0 0.00E+0 int. point 4 2- 10 elastic 4.41E-2 2.51E-1 0.00E+0 7.76E-8 0.00E+0 0.00E+0 0.00E+0 node 21 2- 10 elastic 4.41E-2 2.51E-1 0.00E+0 7.76E-8 0.00E+0 0.00E+0 0.00E+0 node 22 2- 10 elastic 4.41E-2 2.51E-1 0.00E+0 7.76E-8 0.00E+0 0.00E+0 0.00E+0 node 20 2- 10 elastic 4.41E-2 2.51E-1 0.00E+0 7.76E-8 0.00E+0 0.00E+0 0.00E+0 node 19 Example 2: Excerpt from eloutdet file for averaged nodal strain: nodal strain calculations for time step 24 (at time 9.89479E+01 ) node (global) strain eps-xx eps-yy eps-zz eps-xy eps-yz eps-zx 1- lower surface 2.0262E-01 -2.6058E-02 -7.5669E-02 -5.1945E-03 0.0000E+00 0.0000E+00 upper surface 2.0262E-01 -2.6058E-02 -7.5669E-02 -5.1945E-03 0.0000E+00 0.0000E+00 2- lower surface 1.9347E-01 2.3728E-04 -8.3019E-02 -1.4484E-02 0.0000E+00 0.0000E+00 upper surface 1.9347E-01 2.3728E-04 -8.3019E-02 -1.4484E-02 0.0000E+00 0.0000E+00 3- lower surface 2.0541E-01 -5.7521E-02 -6.3383E-02 -1.7668E-03 0.0000E+00 0.0000E+00 upper surface 2.0541E-01 -5.7521E-02 -6.3383E-02 -1.7668E-03 0.0000E+00 0.0000E+00 ⋮ ⋮ ⋮ ⋮ ⋮ ⋮ ⋮ *DATABASE The following cards control content to the d3part binary database (Card 3 is optional). The parameters given here will supercede the corresponding parameters in *DATA- BASE_EXTENT_BINARY when writing the d3part binary database. See also *DATA- BASE_BINARY_D3PART which defines the output interval for d3part and the set of part included in d3part. Card 1 1 2 3 4 5 6 7 8 Variable NEIPH NEIPS MAXINT STRFLG SIGFLG EPSFLG RLTFLG ENGFLG Type Default I 0 I 0 Remarks Card 2 1 2 I 3 1 3 I 0 I 1 I 1 I 1 I 1 4 5 6 7 8 Variable IEVERP SHGE STSSZ I 0 5 I 0 6 7 8 3 4 I 0 2 Type Default Card 3 1 Variable NINTSLD Type Default I NEIPH NEIPS MAXINT STRFLG *DATABASE_EXTENT_D3PART DESCRIPTION Number of additional integration point history variables written to the binary database for solid elements. The integration point data is written in the same order that it is stored in memory-each material model has its own history variables that are stored. For user defined materials it is important to store the history data that is needed for plotting before the data which is not of interest. Number of additional integration point history variables written to the binary database for both shell and thick shell elements for each integration point, see NEIPH above. Number of shell integration points written to the binary database, see also *INTEGRATION_SHELL. If the default value of 3 is used then results are output for the outermost (top) and innermost (bottom) integration points together with results for the neutral axis. If MAXINT is set to 3 and the element has 1 integration point then all three results will be the same. If a value other than 3 is used then results for the first MAXINT integration points in the element will be output. Note: If the element has an even number of integration points and MAXINT is not set to 3 then you will not get mid-surface results. See Remarks below. If MAXINT is set to a negative number, MAXINT integration points are output for each in plane integration point location and no averaging is used. This can greatly increase the size of the binary d3part database. Set to 1 to dump strain tensors for solid, shell and thick shell elements for plotting by LS-PrePost and ASCII file elout. For shell and thick shell elements two tensors are written, one at the innermost and one at the outermost integration point. For solid elements a single strain tensor is written. SIGFLG Flag for including the stress tensor for shells. EQ.1: include (default), EQ.2: exclude. EPSFLG Flag for including the effective plastic strains for shells. EQ.1: include (default), EQ.2: exclude. VARIABLE DESCRIPTION RLTFLG Flag for including stress resultants for shells. EQ.1: include (default), EQ.2: exclude. ENGFLG Flag for including shell internal energy density and shell thickness. EQ.1: include (default), EQ.2: exclude. IEVERP Every plot state for d3part database is written to a separate file. This option will limit the database to 1000 states: EQ.0: more than one state can be on each plot file, EQ.1: one state only on each plot file. SHGE Flag for including shell hourglass energy density. EQ.1: off (default), no hourglass energy written, EQ.2: on. STSSZ Flag for including shell element time step, mass, or added mass. EQ.1: off (default), EQ.2: output time step size, EQ.3: output mass, added mass, or time step size. See remark 3 below. NINTSLD Number of solid element integration points written. The default value is 1. For solids with multiple integration points NINTSLD may be set to 8. Currently, no other values for NINTSLD are allowed. For solids with multiple integration points, an average value is output if NINTSLD is set to 1. *DATABASE_EXTENT_INTFOR The following card controls to some extent the content of the optional intfor binary database. See also *DATABASE_BINARY_INTFOR. The intfor database contains geometry and time history data pertaining to those contact surfaces which are flagged in *CONTACT with the variables SPR and/or MPR. The name of the intfor database must be given on the execution line via “s=filename”. Card 1 1 2 3 4 5 6 7 8 Variable NGLBV NVELO NPRESU NSHEAR NFORC NGAPC NFAIL IEVERF Type Default I 1 I 1 I 1 I 1 I 1 I 1 I 0 I 0 Optional Card. Card 2 1 2 3 4 5 6 7 8 Variable NWEAR NWUSR NHUF Type Default I 0 I 0 I 0 VARIABLE DESCRIPTION NGLBV Output global variables: EQ.-1: no, EQ.1: yes (default). NVELO Output nodal velocity: EQ.-1: no, EQ.1: yes (default). VARIABLE DESCRIPTION NPRESU Output pressures: EQ.-1: no, EQ.1: normal interface pressure (default), EQ.2: normal interface pressure and peak pressure, EQ.3: normal interface pressure, peak pressure and time to peak. NSHEAR Output shear stresses: EQ.-1: no, EQ.1: shear stress in r-direction and s-direction (default). NFORC Output forces: EQ.-1: no, EQ.1: 𝑥-, 𝑦-, 𝑧-force at all nodes (default). NGAPC Output contact gaps at all nodes and surface energy density EQ.-1: no, EQ.1: yes (default). NFAIL Flag for display of deleted contact segments EQ.0: all segments are displayed, EQ.1: remove deleted contact segments from display. IEVERF Every interface force state for the “intfor” database is written to a separate file: EQ.0: more than one interface force state can be on each intfor file, EQ.1: one interface force output state only on each intfor file. NWEAR Output contact wear data, see *CONTACT_ADD_WEAR EQ.0: No output. GE.1: Output wear depth. GE.2: Output sliding distance. NWUSR Number of user wear history variables to output from user defined wear routines, see *CONTACT_ADD_WEAR. Number of user friction history variables to output from user defined friction routines, see *USER_INTERFACE_FRICTION (MPP only). *DATABASE VARIABLE NHUF Remarks: For gaps in Mortar contact, see NGAPC, these are measured with respect to the nominal contact surfaces of the two interacting segments. For instance, if IGNORE = 2 on *CONTACT_...MORTAR then an initial penetration 𝑑 will dislocate the slave contact surface in the negative direction of the slave surface normal 𝒏. The gap 𝑔 reported to the intfor file is still measured between the master and slave surface neglecting this dislocation, thus only physical gaps are reported. Wear outputs are governed by NWEAR and NWUSR, and requires the usage of a wear For NWEAR the “wear depth” model associated with the contact interface. (NWEAR.GE.1) and “sliding distance” (NWEAR.GE.2) are listed under the Nodal fringe menu in LS-PrePost. Following this, NWUSR user defined history variables are listed, corresponding to user wear history variables in a user wear routine. These are listed in the order that they are stored in the wear routine, see WTYPE.LT.0 on *CON- TACT_ADD_WEAR. *DATABASE This keyword controls the content written to the BYU MOVIE databases. See movie option on *DATABASE manual entry. Varriable Cards. Define as many cards as needed. Input ends at next keyword (“*”) card. Card 1 1 2 3 4 5 6 7 8 Variable VTYPE COMP Type I I VARIABLE DESCRIPTION VTYPE Variable type: EQ.0: node, EQ.1: brick, EQ.2: beam, EQ.3: shell, EQ.4: thick shell. COMP . Component components from the following tables can be chosen: the corresponding VTYPE, For ID. integer VTYPE.EQ.0: Table 10.1 , VTYPE.EQ.1: Table 10.2 , VTYPE.EQ.2: not supported, VTYPE.EQ.3: Table 10.3 , VTYPE.EQ.4: not supported. *DATABASE_EXTENT_MPGS Define as many cards as necessary. The created MPGS databases consist of a geometry file and one file for each output database. See MPGS option to *DATABASE keyword. Card 1 1 2 3 4 5 6 7 8 Variable VTYPE COMP Type I I VARIABLE DESCRIPTION VTYPE Variable type: EQ.0: node, EQ.1: brick, EQ.2: beam, EQ.3: shell, EQ.4: thick shell. COMP Component components from the following tables can be chosen: the corresponding VTYPE, For ID. integer VTYPE.EQ.0: Table 14-2 , VTYPE.EQ.1: Table 14-3 , VTYPE.EQ.2: not supported, VTYPE.EQ.3: Table 14-4 , VTYPE.EQ.4: not supported. *DATABASE_EXTENT_SSSTAT_OPTION The only OPTION is: ID The ID option allows the definition of a heading which will be written at the beginning of the ASCII file ssstat. Purpose: This command defines one or more subsystems. A subsystem is simply a set of parts, grouped for convenience. The ASCII output file ssstat provides histories of energy (kinetic, internal, hourglass) and momentum (x, y, and z) for each subsystem. The ssstat file is thus similar to glstat and matsum, but whereas glstat provides data for the whole model and matsum provides data for each individual part, ssstat provides data for each subsystem. The output interval for the ssstat file is given using *DATA- BASE_SSSTAT. To also include histories of subsystem mass properties in the ssstat file, use *DATABASE_SSSTAT_MASS_PROPERTIES. For *DATABASE_EXTENT_BINARY without the ID option, the following card(s) apply. Define as many cards as necessary. Define one part set ID per subsystem, up to 8 subsystems per card. Card 1 1 2 3 4 5 6 7 8 Variable PSID1 PSID2 PSID3 PSID4 PSID5 PSID6 PSID7 PSID8 Type I I I I I I I I For *DATABASE_EXTENT_BINARY_ID option, the following card(s) apply. Define as many cards as necessary. Define one part set ID per subsystem, 1 subsystem per card. Card 1 1 2 3 4 5 6 7 8 Variable PSID1 Type I HEADING1 A70 VARIABLE DESCRIPTION PSIDn Part set ID for subsystem n; see *SET_PART. VARIABLE DESCRIPTION HEADINGn Heading for subsystem n. *DATABASE Purpose: Process FATXML data. FATXML is an open, standardized data format based on the Extensible Markup Language (XML) which is developed by the German Research Association of Automotive Technology (Forschungsvereinigung Automobil- technik - FAT). It is designed for consistent data management in the overall CAE process chain. A comprehensive explanation of the FATXML data format specification is given by Schulte-Frankenfeld and Deiters [2016]. LS-DYNA reads all lines between this keyword and the next keyword recognized by the star (*) sign, processes the data with respect to the include file structure and writes everything together in one output file called ‘d3plot.xml’. Remarks: It is intended that a corresponding FE model consists of one master file with several associated include files each containing a description by *DATABASE_FATXML data, usually at the end of the file. The master file loads the include files via *INCLUDE_- TRANSFORM with potential offset values for nodes, elements, parts, etc. (IDNOFF, IDEOFF, IDPOFF, …). Finally, all data from different include files with different offsets are collected and then summarized in ‘d3plot.xml’. Since the resulting data format is public domain, Post-Processors are able to read that data and correlate it with the associated CAE model. Example: ... *DATABASE_FATXML <?xml version=”1.0”?> <CAE_META_DATA> < PART_ID NAME=”TestCase”> <PDM_DATA> ... <PDD_THICKNESS> < THICKNESS ID=”123”>1.0</THICKNESS > < THICKNESS ID=”124”>1.1</THICKNESS > ... </PDD_THICKNESS > ... </PDM_DATA > </PART_ID > </CAE_META_DATA > *END Purpose: Define the output format for binary files. *DATABASE_FORMAT Card 1 1 2 3 4 5 6 7 8 Variable IFORM IBINARY Type Default Remarks I 0 1 I 0 2 VARIABLE DESCRIPTION IFORM Output format for d3plot and d3thdt files EQ.0: LS-DYNA database format (default), EQ.1: ANSYS database format, EQ.2: Both LS-DYNA and ANSYS database formats. IBINARY Word size of the binary output files (d3plot, d3thdt, d3drlf and interface files for 64 bit computer such as CRAY and NEC. EQ.0: default 64 bit format, EQ.1: 32 bit IEEE format Remarks: 1. The ANSYS output option is not available in MPP and is not universally available in SMP. The LS-DYNA banner in d3hsp will include “ANSYS data- base format” under the list of “Features enabled” if the option is available. 2. By using this option one can reduce the size of the binary output files which are created by 64 bits computer such as CRAY and NEC. *DATABASE_FREQUENCY_ASCII_OPTION Options for frequency domain ASCII databases with the default names given include: NODOUT_SSD ASCII database for nodal results for SSD (displacement, velocity and acceleration). See also *FREQUENCY_DOMAIN_SSD. ELOUT_SSD ASCII database for element results for SSD (stress and strain components). See also *FREQUENCY_DOMAIN_SSD. Card 1 1 2 3 4 5 6 7 8 Variable FMIN FMAX NFREQ FSPACE LCFREQ Type F F Default 0.0 0.0 I 0 I 0 I 0 VARIABLE DESCRIPTION FMIN FMAX Minimum frequency for output (cycles/time) Maximum frequency for output (cycles/time). NFREQ Number of frequencies for output. FSPACE Frequency spacing option for output: EQ.0: linear EQ.1: logarithmic EQ.2: biased LCFREQ Load Curve ID defining the frequencies for output. Remarks: 1. The keyword defines output frequencies for NODOUT_SSD and ELOUT_SSD, and they can be different from output frequencies for D3SSD (which is defined by keyword *DATABASE_FREQUENCY_BINARY_D3SSD). 2. The ASCII databases NODOUT_SSD and ELOUT_SSD are saved in binout files. LS-PREPOST is able to read the binout files directly. Users can also convert these files to ASCII format simply feed them to the l2a program like this: fmin fmin fmin Linear Spacing Logarithmic Spacing fmax fmax mode n mode n+1 mode n+2 Biased Spacing fmax Figure 14-6. Spacing options of the frequency points. l2a binout* 3. The nodes to be output to NODOUT_SSD are specified by card *DATABASE_HISTORY_NODE. 4. The solid, beam, shell and thick shell elements to be output to ELOUT_SSD are specified by the following cards: *DATABASE_HISTORY_SOLID_{OPTION} *DATABASE_HISTORY_BEAM_{OPTION} *DATABASE_HISTORY_SHELL_{OPTION} *DATABASE_HISTORY_TSHELL_{OPTION} 5. There are two methods to define the output frequencies. a) The first method is to define FMIN, FMAX, NFREQ and FSPACE. FMIN and FMAX specify the frequency range of interest and NFREQ specifies the number of frequencies at which results are required. FSPACE speci- fies the type of frequency spacing (linear, logarithmic or biased) to be used. These frequency points for which results are required can be spaced equally along the frequency axis (on a linear or logarithmic scale). Or they can be biased toward the eigenfrequencies (the frequency points are placed closer together at eigenfrequencies in the frequency range) so that the detailed definition of the response close to resonance frequencies can be obtained. b) The second method is to use a load curve (LCFREQ) to define the frequen- cies of interest. *DATABASE_FREQUENCY_BINARY_OPTION Options for frequency domain binary output files with the default names given include: D3ACC D3ACS D3ATV D3FTG D3PSD Binary output file for BEM acoustics (element acoustic pressure contribution and contribution percentage). See also *FREQUEN- CY_DOMAIN_ACOUSTIC_BEM. Binary output file for FEM acoustics (acoustic pressure and sound pressure level). See also *FREQUENCY_DOMAIN_ACOUSTIC_- FEM. Binary output file for acoustic transfer vectors given by BEM acoustic analysis. See also *FREQUENCY_DOMAIN_ACOUSTIC_- BEM_ATV. Binary output file for random vibration fatigue analysis. See also *FREQUENCY_DOMAIN_RANDOM_VIBRATION_FATIGUE. Binary Power Spectral Density output file for random vibration analysis. See also *FREQUENCY_DOMAIN_RANDOM_VIBRA- TION. D3RMS D3SPCM D3SSD Binary Root Mean Square output file for random vibration analysis. See also *FREQUENCY_DOMAIN_RANDOM_VIBRATION. Binary output file for response spectrum analysis. See also *FRE- QUENCY_DOMAIN_RESPONSE_SPECTRUM. Binary output file for steady state dynamics. See also *FREQUEN- CY_DOMAIN_SSD. The D3ACC, D3ACS, D3ATV, D3FTG, D3PSD, D3RMS, D3SPCM and D3SSD files contain plotting information to plot data over the three dimensional geometry of the model. These databases can be plotted with LS-PrePost. • The D3PSD file contains PSD state data for a range of frequencies. The D3SSD file contains state data for a range of frequencies. • For D3SSD, the data can be real or complex, depending on the variable BINARY defined below. • The D3ACC file contains acoustic pressure contribution (and contribution percentage) from each of the boundary elements for a range of frequencies, which are defined in the keyword *FREQUENCY_DOMAIN_ACOUSTIC_BEM. • The D3ACS file contains acoustic results including acoustic pressure and sound pressure level for a range of frequencies, which are defined in the keyword *FRE- QUENCY_DOMAIN_ACOUSTIC_FEM. • The D3FTG, D3RMS and D3SPCM files contain only one state each as they are the data for cumulative fatigue damage ratio, root mean square for random vibration and peak response for response spectrum analysis separately. • The D3ATV file contains NFIELD × NFREQ states, where NFIELD is the number of acoustic field points and NFREQ is the number of output frequencies. Card 1 1 2 3 4 5 6 7 8 Variable BINARY Type Default I - Remarks 1 Additional cards for D3ACC keyword options. Card 2 1 2 3 4 5 6 7 8 Variable NID1 NID2 NID3 NID4 NID5 NID6 NID7 NID8 Type Default I 0 I 0 I 0 I 0 I 0 I 0 I 0 I 0 Additional card for D3PSD and D3SSD keyword options. Card 2 1 2 3 4 5 6 7 8 Variable FMIN FMAX NFREQ FSPACE LCFREQ Type F F Default 0.0 0.0 I 0 I 0 I VARIABLE DESCRIPTION BINARY Flag for writing the binary plot file. EQ.0: Off EQ.1: write the binary plot file EQ.2: write the complex variable binary plot file (D3SSD only) EQ.90: write only real part of frequency response (D3SSD only) EQ.91: write only imaginary part of frequency response (D3SSD only) Field point node ID for writing D3ACC file (up to 10 NID are allowed) Minimum frequency for output (cycles/time) Maximum frequency for output (cycles/time). NID1,… FMIN FMAX NFREQ Number of frequencies for output. FSPACE Frequency spacing option for output: EQ.0: linear EQ.1: logarithmic EQ.2: biased LCFREQ Load Curve ID defining the frequencies for output. Remarks: fmin fmin fmin Linear Spacing Logarithmic Spacing fmax fmax mode n mode n+1 mode n+2 Biased Spacing fmax Figure 14-7. Spacing options of the frequency points. 1. For OPTION = D3SSD, If BINARY = 1, only the magnitude of the displacement, velocity, acceleration and stress response is written into the binary database “d3ssd” which can be accessed by LS-PrePost 3.0 or older versions. For cus- tomers using LS-PrePost 3.0 or older versions, it is suggested to set BINARY = 1. If BINARY = 2, both the magnitude and the phase angle of the response are written into “d3ssd” so that LS-PrePost (3.1 or higher versions) can run modal expansion (to show the cyclic time history fringe plot) on each output frequen- cy. If BINARY = 90 or 91, only real or imaginary part of the response is written into “d3ssd”. 2. There are two methods to define the output frequencies. a) The first method is to define FMIN, FMAX, NFREQ and FSPACE. FMIN and FMAX specify the frequency range of interest and NFREQ specifies the number of frequencies at which results are required. FSPACE speci- fies the type of frequency spacing (linear, logarithmic or biased) to be used. These frequency points for which results are required can be spaced equally along the frequency axis (on a linear or logarithmic scale). Or they can be biased toward the eigenfrequencies (the frequency points are placed closer together at eigenfrequencies in the frequency range) so that the detailed definition of the response close to resonance frequencies can be obtained. b) The second method is to use a load curve (LCFREQ) to define the frequen- cies of interest. *DATABASE Purpose: When a Lagrangian mesh overlaps with an Eulerian or ALE mesh, the fluid- structure (or ALE-Lagrangian) interaction is often modeled using the *CON- STRAINED_LAGRANGE_IN_SOLID card. This keyword (*DATABASE_FSI) causes certain coupling information related to the flux through and load on selected Lagrangian surfaces defined in corresponding *CONSTRAINED_LAGRANGE_IN_- SOLID card to be written to the ASCII-based dbfsi file or in the case of MPP-DYNA the binout file. NOTE: This card must be associated with a *CON- STRAINED_LAGRANGE_IN_SOLID penalty meth- od coupling. This card is not compatible with constrained-based coupling. Card 1 1 2 3 4 5 6 7 8 Variable DTOUT Type F Surface Card. Add one card per surface. This input terminates at the next keyword (“*”) card. Card 2 1 2 3 4 5 6 7 8 Variable DBFSI_ID SID SIDTYPE SWID CONVID NDSETID CID Type I I I I I I I VARIABLE DESCRIPTION DTOUT Output interval time step DBFSI_ID Surface ID (for reference purposes only) or a DATABASE_FSI entity ID. It consists of a geometric entity defined by the SID below. SID *DATABASE_FSI DESCRIPTION Set ID defining the geometrical surface(s) through which or upon which some data is to be tracked and output to a file called “dbfsi”. This set ID can be a (1) PID or (2) PSID or (3) SGSID. This Lagrangian SID must be contained in a Lagrangian slave SID defined in a corresponding coupling card, *CONSTRAINED_LA- GRANGE_IN_SOLID. SIDTYPE Set type: EQ.0: Part set EQ.1: Part EQ.2: Segment set SWID CONVID This is an ID from a corresponding *ALE_FSI_SWITCH_MMG_- ID card. This card allows for the AMMG ID of an ALE material to be switched as it passes across a monitoring surface. If defined, the accumulative mass of the “switched” ALE multi- material group (AMMG) is written out under the “mout” parameter in the “dbfsi” file. This is used mostly for airbag application only: CONVID is an ID from a corresponding *LOAD_ALE_CONVECTION_ID card which computes the heat transfer between inflator gas (ALE material) and the inflator canister (Lagrangian part). If defined, the temperature of the Lagrangian part having heat transfer with the gas, and its change in temperature as function of time are output in the “dbfsi” file. NDSETID Set ID consisting of the nodes on which the moments of the forces applied on SID are computed. See Remark 3. CID Coordinate system ID, see *DEFINE_COORDINATE_SYSTEM. Remarks: 1. Overview of dbfsi File. The dbfsi parameters output are enumerated below. pres = Averaged estimated coupling pressure over each surface entity being monitored. For example, if using SI base units for mass- length-time-temperature, this pressure would then be in Pascal. fx, fy, fz = Averaged total estimated coupling force components (N in met- ric units) along the global coordinate directions, over each sur- face entity defined, and acting at the centroid of each surface. mout = Accumulated mass (Kg in metric units) passing through each DBFS_ID surface entity. See Remark 2 below. (This parameter used to be called “pleak”). obsolete = (This parameter used to be called “mflux”). gx, gy, gz = Average estimated leakage-control force component over the surface entity. This data is useful for debugging. Leakage con- trol forces are too large (relative to the main coupling forces, fx, fy and fz) may indicate that alternate coupling approach should be considered since the main coupling force is putting out too little resistance to leakage. (These parameters used to be called fx-lc, fy-lc and fz-lc). Ptmp = Lagrangian part Temperature (Activated only when the *LOAD_ALE_CONVECTION card is used). PDt = Lagrangian part Temperature change (Activated only when the *LOAD_ALE_CONVECTION card is used). 2. MOUT. “mout” parameter in the “dbfsi” output from this keyword contains the accumulated mass passing through each DBFS_ID surface entity. For 4 different cases: a) When LCIDPOR is defined in the coupling card (CLIS), porous accumu- lated mass transport across a Lagrangian shell surface may be monitored and output in “mout”. b) Porous flow across Lagrangian shell may also be defined via a load curve in the *MAT_FABRIC card, and similar result will be tracked and output. This is an alternate form of (a). c) When NVENT in the CLIS card is defined (isentropic venting), the venting mass transport across the isentropic vent hole surface may be output in “mout”. d) When an *ALE_FSI_SWITCH_MMG_ID card is defined, and the SWID parameter specifies this ID to be tracked, then the amount of accumulated mass that has been switched when passing across a monitoring surface is output. 3. Calculation of Moments for NDSETID. A geometrical surface SID has a centroid where the coupling forces are averaged. The distances between this centroid and the nodes defined by the set NDSETID are the lever arms. The moments are the cross-products of these distances with the averaged coupling forces. For each node in the set NDSETID, a new line in the “dbfsi” file is in- serted after each output for the corresponding coupling forces . These additional lines have the format following the template established by the example in Remark 1 where the forces are replaced by the moments and the node ID replaces the DBFSI_ID values. Example: Consider a model with a Lagrangian mesh overlaps with an Eulerian or ALE mesh. On the Lagrangian mesh, there are 3 Lagrangian surface sets over which some data is to be written out. $...|....1....|....2....|....3....|....4....|....5....|....6....|....7....|....8 $ INPUT: $...|....1....|....2....|....3....|....4....|....5....|....6....|....7....|....8 *DATABASE_FSI $ dt 2.97E-06 $ DBFSI_ID SID STYPE swid convid [STYPE: 0=PSID;1=PID;2=SGSID] 11 1 2 12 2 2 13 3 1 $...|....1....|....2....|....3....|....4....|....5....|....6....|....7....|....8 $ This reads: $ DBFSI_ID 11 is defined by a SID=1: a SGSID = as specified by STYPE=2 $ DBFSI_ID 12 is defined by a SID=2: a SGSID = as specified by STYPE=2 $ DBFSI_ID 13 is defined by a SID=3: a PID = as specified by STYPE=1 $...|....1....|....2....|....3....|....4....|....5....|....6....|....7....|....8 $ An OUTPUT file called “dbfsi” looks like the following: $...|....1....|....2....|....3....|....4....|....5....|....6....|....7....|....8 Fluid-structure interaction output Number of surfaces: 3 id pres fx fy fz mout obsolete gx gy gz Ptmp PDt time= 0.00000E+00 11 0.0000E+00 0.0000E+00 0.0000E+00 0.0000E+00 0.0000E+00 0.0000E+00 0.0000E+00 0.0000E+00 0.0000E+00 0.0000E+00 0.0000E+00 12 0.0000E+00 0.0000E+00 0.0000E+00 0.0000E+00 0.0000E+00 0.0000E+00 0.0000E+00 0.0000E+00 0.0000E+00 0.0000E+00 0.0000E+00 13 0.0000E+00 0.0000E+00 0.0000E+00 0.0000E+00 0.0000E+00 0.0000E+00 0.0000E+00 0.0000E+00 0.0000E+00 0.0000E+00 0.0000E+00 time= 0.29709E-05 11 0.0000E+00 0.0000E+00 0.0000E+00 0.0000E+00 0.0000E+00 0.0000E+00 0.0000E+00 0.0000E+00 0.0000E+00 0.0000E+00 0.0000E+00 12 0.0000E+00 0.0000E+00 0.0000E+00 0.0000E+00 0.0000E+00 0.0000E+00 0.0000E+00 0.0000E+00 0.0000E+00 0.0000E+00 0.0000E+00 13 0.0000E+00 0.0000E+00 0.0000E+00 0.0000E+00 0.0000E+00 0.1832E-06 0.0000E+00 0.0000E+00 0.0000E+00 0.0000E+00 0.0000E+00 $...|....1....|....2....|....3....|....4....|....5....|....6....|....7....|....8 *DATABASE_FSI_SENSOR Purpose: This card activates the output of an ASCII file called “dbsensor”. Its input defines the pressure sensors’ locations which follow the positions of some Lagrangian segments during the simulation. Its ASCII output file, dbsensor, contains the spatial position of the sensor and its recorded pressure from the ALE elements containing the sensors. This card is activated when a *CONSTRAINED_LAGRANGE_IN_SOLID card is used and the Lagrangian shell elements defining the locations of the sensors must be included in the slave or structure coupling set. 2 3 4 5 6 7 8 Card 1 Variable 1 DT Type F Surface Card. Add one card per surface. This input terminates at the next keyword (“*”) card. Card 1 2 3 4 5 6 7 8 Variable DBFSI_ID NID SEGMID OFFSET ND1 ND2 ND3 Type I I I F I I I VARIABLE DESCRIPTION DT Output interval DBFSI_ID Pressure-Sensor ID. NID SEGMID An optional Lagrangian node ID defining an approximate pressure sensor location with respect to a Lagrangian shell element. This is not a required input. A required Lagrangian element ID for locating the pressure sensor. If NID = 0 or blank, the sensor will be automatically placed in the center of this SEGMID, accounting for the offset distance. If the model is 3D, the Lagrangian element can be a shell or solid (for this latter, ND1 and ND2 are required to define the face). If the model is 2D, the Lagrangian element can be a beam or shell (for this latter, ND1 and ND2 are required to define the side). DESCRIPTION Offset distance between the pressure sensor and the Lagrangian segment surface. If it is positive, it is on the side pointed to by the segment normal vector and vice versa. Nodes defining the solid face in 3D or shell side in 2D, from which the sensor is located. In 3D, if the solid face has 4 nodes, only the diagonal opposites ND1 and ND2 are required. If the solid face is triangular, a third node ND3 should be provided. In 2D, only ND1 and ND2 are required to define the shell side. VARIABLE OFFSET ND1, ND2, ND3 Remarks: 1. The output parameters in the “dbsensor” ASCII file are: ID = Sensor ID. x, y, z = Sensor spatial location. P = Sensor recorded pressure (Pa) from the ALE fluid element con- taining the sensor. For example, to plot the sensor pressure in LS-Prepost, select: ASCII → dbsensor → LOAD → (select sensor ID) → Pressure → PLOT Example 1: $...|....1....|....2....|....3....|....4....|....5....|....6....|....7....|....8 $ INPUT: $...|....1....|....2....|....3....|....4....|....5....|....6....|....7....|....8 *DATABASE_FSI_SENSOR 0.01 $ DBFSI_ID NID SEGMENTID OFFSET 10 360 355 -0.5 20 396 388 -0.5 30 324 332 -0.5 $...|....1....|....2....|....3....|....4....|....5....|....6....|....7....|....8 $ The 1st line reads: $ SENSOR_ID 10 is located by segment-ID=355. Node-ID=360 precisely locate this $ sensor (if NID=0, then the sensor is located at the segment center). This $ sensor is located 0.5 length unit away from the segment surface. Negative $ sign indicates a direction opposite to the segment normal vector. $...|....1....|....2....|....3....|....4....|....5....|....6....|....7....|....8 $ An OUTPUT file called “dbsensor” looks like the following: $...|....1....|....2....|....3....|....4....|....5....|....6....|....7....|....8 ALE sensors output Number of sensors: 3 id x y z p time= 0.17861E-02 10 0.0000E+00 0.0000E+00 -0.3900E+00 0.1085E-03 20 -0.2250E+02 0.2250E+02 -0.3900E+00 0.1085E-03 30 0.2250E+02 -0.2250E+02 -0.3900E+00 0.1085E-03 time= 0.20081E-02 10 0.0000E+00 0.0000E+00 -0.3900E+00 0.1066E-03 20 -0.2250E+02 0.2250E+02 -0.3900E+00 0.1066E-03 30 0.2250E+02 -0.2250E+02 -0.3900E+00 0.1066E-03 $...|....1....|....2....|....3....|....4....|....5....|....6....|....7....|....8 $ ID = DBFSI_ID $ x,y,z = Sensor location (defined based on a Lagrangian segment) $ p = Sensor pressure as taken from the fluid element containing the sensor. $...|....1....|....2....|....3....|....4....|....5....|....6....|....7....|....8 Available options include: *DATABASE BEAM BEAM_SET BEAM_ID DISCRETE DISCRETE_ID DISCRETE_SET NODE NODE_ID NODE_LOCAL NODE_LOCAL_ID NODE_SET NODE_SET_LOCAL SEATBELT SEATBELT_ID SHELL SHELL_ID SHELL_SET SOLID SOLID_ID SOLID_SET SPH SPH_SET TSHELL TSHELL_ID *DATABASE_HISTORY Purpose: Control which nodes or elements are output into the binary history file, d3thdt, the ASCII file nodout, the ASCII file elout and the ASCII file sphout. Define as many cards as necessary. The next “*” card terminates the input. See also *DATA- BASE_BINARY_OPTION and *DATABASE_OPTION. Node/Element Cards for Case I (no “ID”, and no “LOCAL”). Cards for keyword options BEAM, BEAM_SET, DISCRETE, DISCRETE_SET, NODE, NODE_SET, SEAT- BELT, SHELL, SHELL_SET, SOLID, SOLID_SET, SPH, SPH_SET, TSHELL, and TSHELL_SET. Include as many as needed. Input terminates at the next keyword (“*”) card. Card 1 1 Variable ID1 2 ID2 3 ID3 4 ID4 5 ID5 6 ID6 7 ID7 8 ID8 Type I I I I I I I I VARIABLE IDn DESCRIPTION NODE/NODE_SET or element/element set ID n. Elements may be BEAM/BEAM_SET, DISCRETE/DISCRETE_SET, SEATBELT, TSHELL/ SHELL/SHELL_SET, TSHELL_SET. The contents of the files are given in Table 14-2 for nodes, Table 14-3 for solid elements, Table 14-4 for shells and thick shells, and Table 14-5 for beam elements. In the binary file, D3THDT, the contents may be extended or reduced with the *DATABASE_EXTENT_BINARY definition. SOLID/SOLID_SET, or Node/Element Cards for Case II (“ID” option, but no “LOCAL”). Cards for keyword options BEAM_ID, NODE_ID, SEATBELT_ID, SHELL_ID, SOLID_ID, and TSHELL_ID. Include as many as needed. Input terminates at the next keyword (“*”) card. Card 1 Variable 1 ID Type I 2 3 4 5 6 7 8 HEADING A70 VARIABLE DESCRIPTION ID Node or element ID VARIABLE HEADING DESCRIPTION A description of the node or element. It is suggested that unique descriptions be used. This description is written into the D3HSP file and into the ASCII databases nodout and elout. Node Cards for Case III (“LOCAL” option). Card 1 for keyword options NODE_LO- CAL, NODE_LOCAL_ID, and NODE_SET_LOCAL. Include as many cards as needed to specify all the nodes. This input terminates at the next keyword (“*”) card. Card 1 Variable 1 ID 2 3 4 5 6 7 8 CID REF HFO Type I I I I ID Card for Case III. Additional card for ID option. This card is only used for the NODE_LOCAL_ID keyword option. When activated, each node is specified by a pair of cards consisting of “Card 1,” and, secondly, this card. Include as many pairs as needed to specify all the nodes. This input terminates at the next keyword (“*”) card. Card 2 1 2 3 4 5 6 7 8 Variable Type HEADING A70 VARIABLE DESCRIPTION ID CID NODE/NODE_SET set ID. The contents of the files are given in Table 14-2 for nodes. See the remark below concerning accelerometer nodes. Coordinate system ID for nodal output. See DEFINE_COORDI- NATE options. REF *DATABASE_HISTORY DESCRIPTION Output coordinate system for displacements, velocities, and accelerations. (Nodal coordinates are always in the global coordinate system.) EQ.0: Output is in the local system fixed for all time from the beginning of the calculation. If CID is nonzero, FLAG in the corresponding *DEFINE_COORDINATE_NODES command must be set to 0. FLAG has no bearing on results when REF is set to 1 or 2. EQ.1: Translational output is the projection of the node’s absolute translational motion onto the local system. The local system is defined by the *DEFINE_COORDI- NATE_NODES command and can change orientation according to the movement of the three defining nodes. The defining nodes can belong to either deformable or rigid parts. EQ.2: Translational output is the projection of the node’s relative translational motion onto the local system. Here, “relative” means relative to node N1 of that local system. In other words, the displacement of the origin (node N1) of the local coordinate system is first subtracted from the displacement of the node of interest before projecting it onto the translating and rotating local coordinate system. The local system is defined as described in REF = 1 above. If dynamic relaxation is used, the reference loca- tion is reset when convergence is achieved. Rotational output is truly relative to the updated location coordi- nate system only if REF = 2. HFO Flag for high frequency output into nodouthf EQ.0: Nodal data written to nodout file only EQ.1: Nodal data also written nodouthf at the higher frequency HEADING A description of the nodal point. It is suggested that unique description be used. This description is written into the d3hsp file and into the ASCII database nodout. Remarks: 1. If a node belongs to an accelerometer, see *ELEMENT_SEATBELT_AC- CELEROMETER, and if it also appears as an active node in the NODE_LOCAL or NODE_SET_LOCAL keyword, the coordinate system, CID, transformations will be skipped and the LOCAL option will have no effect. *DATABASE_MASSOUT Purpose: Output nodal masses into ASCII file MASSOUT. Card 1 1 2 3 4 5 6 7 8 Variable SETID NDFLG RBFLG Type Default I 0 I 1 I 0 VARIABLE DESCRIPTION SETID Optional set ID. EQ.0: mass output for all nodes, LT.0: no output, GT.0: set ID identifying nodes whose mass will be output. NDFLG Database extent: EQ.1: output translational mass identified by SETID (default), for deformable nodes EQ.2: output translational mass and rotary inertias for the deformable nodes identified by the SETID. EQ.3: output translational mass for deformable and rigid nodes identified by SETID (default), EQ.4: output translational mass and rotary inertias for the deformable and rigid nodes identified by the SETID. RBFLG Rigid body data: EQ.0: no output for rigid bodies, EQ.1: output rigid body mass and inertia. Remarks: 1. Nodes and rigid bodies with no mass are not output. By inference, when the set ID is zero and no output shows up for a node, then the mass of that node is zero. *DATABASE_NODAL_FORCE_GROUP Purpose: Define a nodal force group for output into the ASCII file nodfor. The output interval must be specified using *DATABASE_NODFOR . Card 1 1 2 3 4 5 6 7 8 Variable NSID CID Type I I Default none none VARIABLE DESCRIPTION Nodal set ID, see *SET_NODE_OPTION. Coordinate system ID for output of data in local system, NSID CID Remarks: 1. The reaction forces in the global 𝑥, 𝑦, and 𝑧 directions (and local 𝑥, 𝑦, and 𝑧 directions if CID is defined above) for the nodal force group are written to the nodfor file along with the external work done by these reaction forces. The reaction forces in the global 𝑥, 𝑦, and 𝑧 directions for each node in the nodal force group are also written to nodfor. These forces can be a result of applied boundary forces such as nodal point forces and pressure boundary conditions, body forces, and contact interface forces. In the absence of body forces, interior nodes would always yield a null force resultant vector. In general this option would be used for surface nodes. *DATABASE_PAP_OUTPUT Purpose: Set contents of output files for pore air pressure calculations. Card 1 1 2 3 4 5 6 7 8 Variable IVEL IACCX IACCY IACCZ NCYOUT Type Default I 0 I 0 I 0 I 0 I 100 VARIABLE DESCRIPTION IVEL Meaning of “Velocity” in d3plot and d3thdt output files EQ.0: Nodal velocity vector EQ.1: Seepage velocity vector IACCX, Y, Z Meaning of “X/Y/Z-Acceleration” in d3plot and d3thdt output files EQ.0: Not written EQ.21: Nodal air density EQ.22: Nodal pore air pressure EQ.24: Nodal air mass EQ.25: Nodal air mass flow rate NCYOUT Number of cycles between outputs of calculation status to d3hsp and log files *DATABASE Purpose: Plot the distribution or profile of a data along x, y, or z-direction. Card 1 Variable 1 DT Type I 2 ID I 3 4 5 6 7 8 TYPE DATA DIR UPDLOC MMG I I I I 0 I 0 Default none none none none none VARIABLE DESCRIPTION DT ID Interval time. Set ID. TYPE Set type: EQ.1: Node Set, EQ.2: Solid Set, EQ.3: Shell Set, EQ.4: Segment Set, EQ.5: Beam Set. DATA Data type: EQ.1: 𝑥-velocity, EQ.2: 𝑦-velocity, EQ.3: 𝑧-velocity, EQ.4: velocity magnitude, EQ.5: 𝑥-acceleration, EQ.6: 𝑦-acceleration, EQ.7: 𝑧-acceleration, EQ.8: acceleration magnitude, EQ.9: pressure, EQ.10: 𝑥𝑥-stress, VARIABLE DESCRIPTION EQ.11: 𝑦𝑦-stress, EQ.12: 𝑧𝑧-stress, EQ.13: 𝑥𝑦-stress, EQ.14: 𝑦𝑧-stress, EQ.15: 𝑧𝑥-stress, EQ.16: temperature, EQ.17: volume fraction, EQ.18: kinetic energy, EQ.19: internal energy, EQ.20: density. DIR Direction: EQ.1: 𝑥-direction, EQ.2: 𝑦-direction, EQ.3: 𝑧-direction, EQ.4: Curvilinear (relative distances between elements of set ID are added up in the order defined by the set) UPDLOC Flag to update the set location: EQ.0: Only the initial position of set ID is considered EQ.1: The positions of the elements composing the set are updated each DT MMG Multi-Material ALE group id. See Remark 2. GT.0: Multi-Material ALE group id LT.0: |MMG| is the id of a *SET_MULTI-MATERIAL_- GROUP_LIST that can list several Multi-Material ALE group ids. Remarks: 1. At a given time 𝑇 the profile is written in a file named profile_DATA_- DIR_timeT.xy (DATA and DIR are replaced by the data and direction names respectively). The file has a xyplot format that LS-PrePost can read and plot. For example, DATA = 9, DIR = 2 and DT = 0.1 sec will save a pressure profile at 𝑡 = 0.0 sec in profile_pressure_y_time0.0.xy, at 𝑡 = 0.1 sec in profile_pressure_y_ time0.1.xy, at 𝑡 = 0.2 sec in profile_pressure_y_time0.2.xy. 2. In the case of a multi-material ALE model (elform = 11 in *SECTION_SOLID or *SECTION_ALE2D or *SECTION_ALE1D), an element can contain several materials with each material being associated with its own pressures and stresses. It is the default behavior for volume averaging to be applied to ele- ment data before being written out; however, when the multi-material group field, MMG, is set, then element data are output only for the specified materials. *DATABASE_PWP_FLOW Purpose: Request output containing net inflow of fluid at a set of nodes. Card 1 1 2 3 4 5 6 7 8 Variable NSET Type Default I 0 VARIABLE DESCRIPTION NSET Node set ID Remarks: Any number of these cards can be used. Nett inflow or outflow arises when maintaining an applied PWP boundary condition implies addition or removal of water. Output is written to a file named database_pwp_flow.csv, a comma-separated ascii file. Each line consists of (time, flow1, flow2, …) where flow1 is the total inflow at the node set for the first DATABASE_PWP_FLOW request, flow2 is for the second, etc. *DATABASE Purpose: Set contents of output files for pore pressure calculations. Card 1 1 2 3 4 5 6 7 8 Variable IVEL IACCX IACCY IACCZ NCYOUT Type Default I 0 I 0 I 0 I 0 I 100 VARIABLE DESCRIPTION IVEL Meaning of “Velocity” in d3plot and d3thdt output files EQ.0: Nodal velocity vector EQ.1: Seepage velocity vector IACCX, Y, Z Meaning of “X/Y/Z-Acceleration” in d3plot and d3thdt output files EQ.0: Not written EQ.1: Total pwp head EQ.2: Excess pwp head (this is also written as temperature) EQ.3: Target rate of volume change EQ.4: Actual rate of volume change EQ.7: Hydraulic pwp head EQ.8: Error in rate of volume change (calculated from seepage minus actual) EQ.9: Volume at node EQ.10: Rate of volume change calculated from seepage EQ.14: Void volume (generated at suction limit) EQ.17: NFIXCON (e.g: +4/-4 for nodes on suction limit) NCYOUT Number of cycles between outputs of calculation status to d3hsp, log, and tdc_control_output.csv files (time-dependent and steady-state analysis types). *DATABASE_RCFORC_MOMENT Purpose: Define contact ID and nodes for moment calculations. Moments are written to rcforc according to output interval given in *DATABASE_RCFORC. If *DATA- BASE_RCFORC_MOMENT is not used, the moments reported to rcforc are about the origin (0, 0, 0). Card 1 1 2 3 4 5 6 7 8 Variable CID NODES NODEM Type I I I VARIABLE DESCRIPTION CID Contact ID NODES NODEM Node about which moments are calculated due to contact forces on slave surface. Node about which moments are calculated due to contact forces on master surface. *DATABASE Purpose: Recovers the stresses at nodal points of solid or thin shell elements by using Zienkiewicz-Zhu’s Superconvergent Patch Recovery method. 5 6 7 8 Card 1 1 Variable PSID Type Default I 0 2 IAX A 0 3 IAY A 0 4 IAZ A 0 VARIABLE PSID DESCRIPTION Part set ID of solid or thin shell elements whose nodal stress will be recovered IAX, IAY, IAZ Meaning of “𝑥/𝑦/𝑧-Acceleration” in d3plot and d3thdt output files EQ.SMNPD: the minimum principal deviator stress EQ.SMNPR: the minimum principal stress EQ.SMXPD: the maximum principal deviator stress EQ.SMXPR: the maximum principal stress EQ.SMXSH: the maximum shear stress EQ.SPR: nodal pressure EQ.SVM: nodal von Mises stress EQ.SXX: EQ.SYY: EQ.SZZ: EQ.SXY: EQ.SYZ: EQ.SZX: nodal normal stress along 𝑥 direction nodal normal stress along 𝑦 direction nodal normal stress along 𝑧 direction nodal shear stress along 𝑥-𝑦 direction nodal shear stress along 𝑦-𝑧 direction nodal shear stress along 𝑧-𝑥 direction For shell elements append either “B” or “T” to the input string to recover nodal stresses at the bottom or top layer of shell elements. For example, SPRT recovers the nodal pressure at the top layer. *DATABASE_RECOVER_NODE 1. Recovered stresses are in global coordinate system. *DATABASE_SPRING_FORWARD Purpose: Create spring forward nodal force file. This option is to output resultant nodal force components of sheet metal at the end of the forming simulation into an ASCII file, “SPRING-FORWARD”, for spring forward and die corrective simulations. Card 1 1 2 3 4 5 6 7 8 Variable IFLAG Type I VARIABLE DESCRIPTION IFLAG Output type: EQ.0: off, EQ.1: output element nodal force vector for deformable nodes. *DATABASE_SUPERPLASTIC_FORMING Purpose: Specify the output intervals to the superplastic forming output files. The option *LOAD_SUPERPLASTIC_FORMING must be active. Card 1 1 2 3 4 5 6 7 8 Variable DTOUT Type F VARIABLE DTOUT DESCRIPTION Output time interval for output to “pressure”, “curve1” and “curve2” files. The “pressure” file contains general information from the analysis and the files “curve1” and “curve2” contain pressure versus time from phases 1 and 2 of the analysis. The data in the pressure and curve files may be plotted using ASCII → superpl in LS-PrePost. *DATABASE Purpose: Tracer particles will save a history of either a material point or a spatial point into an ASCII file: trhist. This history includes positions, velocities, and stress components. The option *DATABASE_TRHIST must be active. This option applies to ALE, SPH and DEM (Discrete Element Method) problems. Available options are: <BLANK> DE The DE option defines a tracer corresponding to discrete elements (*ELEMENT_DIS- CRETE_SPHERE) . See Remarks 2 and 4. Card 1 2 Variable TIME TRACK Type F Default 0.0 I 0 3 X F 0 4 Y F 0 5 Z F 0 6 7 8 AMMGID NID RADIUS I 0 I 0 F 0.0 VARIABLE DESCRIPTION TIME Start time for tracer particle TRACK Tracking option: EQ.0: particle follows material, EQ.1: particle is fixed in space. X Y Z Initial 𝑥-coordinate Initial 𝑦-coordinate Initial 𝑧-coordinate AMMGID The AMMG ID (ALE multi-material group) of the material being tracked in a multi-material ALE element. See Remark 1. NID *DATABASE_TRACER DESCRIPTION An optional node ID defining the initial position of a tracer particle. If defined, its coordinates will overwrite the 𝑥, 𝑦, 𝑧 coordinates above. This feature is for TRACK = 0 only and can be applied to ALE tracers and DE tracers. See Remark 2. RADIUS Radius is used only for the DE option to indicate whether the tracer follows and monitors a single discrete element or multiple discrete elements. GT.0: The tracer takes the average results of all discrete elements located inside a sphere with radius = RADIUS. That sphere stays centered on the DE tracer. LT.0: The discrete element closest to the tracer is used. The magnitude of RADIUS in this case is unimportant. Remarks: 1. Multi-Material Groups. ALE elements can contain multi-materials. Each material is referred to as an ALE multi-material group or AMMG. Each AMMG has its list of history variables that can be output. For example, if a tracer is in a mixed element consisting of 2 AMMGs, and the history variables of AMMG 1 are to be output or tracked, the AMMGID should be defined as AMMGID=1. If AMMGID=0, a volume-fraction-weighted-averaged pressure will be reported instead. 2. NID Description. For ALE, NID is a massless dummy node. Its location will be updated according to the motion of the ALE material. For the DE option, NID is a discrete element node that defines the initial loca- tion of the tracer. The DE tracer continues to follow that node if RADIUS < 0. On the other hand, the DE tracer’s location is updated according to the average motion of the group of DE nodes inside the sphere defined by RADIUS when RADIUS > 0. 3. Tracer particles in ambient ALE elements. Since the auxiliary variables (6 stresses, plastic strain, internal energy, …) for ambient elements are reset to their initial values before and after advection and tracer data are stored in trhist during the advection cycle, tracers in ambient elements show the initial stresses, not the current ones. 4. Discrete Elements. If _DE is used, tracer particles will save a history of either a material point or a spatial point into an ASCII file: demtrh. This history in- cludes positions, velocities components, stress components, porosity, void ratio, and coordination number. The option *DATABASE_TRHIST must be active. *DATABASE_TRACER_GENERATE Purpose: Generate tracer particles along an isosurface for a variable defined in the VALTYPE list. The tracer particles follow the motion of this surface and save data histories into a binary file called trcrgen_binout . These histories are identical to the ones output by *DATABASE_TRACER into the trhist file. They include positions, velocities, and stress components. Except for the positions and element id specifying where the tracer is, the output can be controlled with the VARLOC and VALTYPE2 fields. This option applies to ALE problems. Card 1 1 2 3 4 5 6 7 8 Variable DT VALOW VALUP VALTYPE1 SET SETYPE MMGSET UPDT Type F F F I Default none 0.0 0.0 none I 0 I 0 I F none 0.0 Optional Variable Cards. Cards defining new variables to be output to t trcrgen_binout instead of the default ones. Include as many cards as necessary. This input ends at the next keyword (“*”) card. Card 2 1 2 3 4 5 6 7 8 Variable VARLOC VALTYPE2 MMGSET Type Default I 0 I 0 I 0 VARIABLE DT VALOW, VALUP DESCRIPTION Interval time between each tracer generation and position update . Range of values between which the isosurface is defined. VALOW is the lower bound while VALUP is the upper bound. See Remark 2. The value at the isosurface is 0.5(VALOW + VALUP). The variable with this value is defined by VALTYPE. VARIABLE VALTYPE1 VALTYPE2 DESCRIPTION The variable that will be used to generate the isosurfaces. See VALTYPE2 for enumeration of values. Data to be output to the trcrgen_binout file. The interpretation of VALTYPE1 and VALTYPE2 is enumerated in the following list: EQ.1: EQ.2: EQ.3: EQ.4: EQ.5: EQ.6: EQ.7: EQ.8: EQ.9: EQ.10: 𝑥𝑥-stress 𝑦𝑦-stress 𝑧𝑧-stress 𝑥𝑦-stress 𝑦𝑧-stress 𝑧𝑥-stress plastic strain internal energy bulk viscosity relative volume GE.11 and LE.19: other auxiliary variables EQ.20: EQ.21: EQ.22: EQ.23: EQ.24: EQ.25: EQ.26: EQ.27: EQ.28: EQ.29: EQ.30: EQ.31: EQ.31: EQ.33: EQ.34: pressure density material volume compression ratio element volume fraction nodal volume fraction 𝑥-position 𝑦-position 𝑧-position 𝑥-velocity 𝑦-velocity 𝑧-velocity velocity 𝑥-acceleration 𝑦- acceleration *DATABASE_TRACER_GENERATE EQ.35: EQ.36: EQ.37: EQ.38: DESCRIPTION 𝑧- acceleration acceleration nodal mass nodal temperature SET Set ID SETYPE Type of set : EQ.0: EQ.1: EQ.2: solid set segment set node set MMGSET Multi-material group set . UPDT Time interval between tracer position update . VARLOC Variable location in trcrgen_binout to be replaced with the variable specified in the VALTYPE2 field: EQ.4: EQ.5: EQ.6: EQ.7: EQ.8: EQ.9: EQ.10: EQ.11: EQ.12: EQ.13: EQ.14: EQ.15: 𝑥-velocity 𝑦-velocity 𝑧-velocity 𝑥𝑥-stress 𝑦𝑦-stress 𝑧𝑧-stress 𝑥𝑦-stress 𝑦𝑧-stress 𝑧𝑥-stress plastic strain density relative volume Remarks: 1. DT. The frequency to create tracers is defined by DT. The default value of UPDT, which is the time interval between updates to the tracer position, is also set to DT. The default behavior, then, is to update tracer positions when a new tracer is created, however, by setting UPDT to a value less than DT tracer posi- tions can be updated more frequently without creating new tracers. 2. Tracing Algorithm. When LS-DYNA adds new tracer particles tracers are created at element centers, segment centers, or nodes depending on the set type (SETYPE). A new tracer particle is created when the value at the element center, segment center, or node center is in the bounding interval [VALOW, VALUP], provided that there is not already a nearby tracer particle. The tracer particles follow the iso-surface defined by the midpoint of the bounding inter- val (VALOW + VALUP)/2. 3. Multi-Material Groups. ALE elements can contain several materials. Each material is referred to as an ALE multi-material group. The volume fractions define how much of the element volume is occupied by the groups. Each group has their own variables for 0<VALTYPE<26. IF VALTYPE<21 or VALTYPE=23, the variable is volume averaged over the groups defined by MMGSET. 4. Post-Procesing. The output of *DATABASE_TRACER_GENERATE is written to a file named trcrgen_binout. To access the output in LS-PrePost: [TAB 2] → [LOAD] → [trcrgen_binout] → [trhist] → “Trhist Data” window contains a list of variables output for each tracer. 5. Binary to ASCII File Conversion. The variables in trhist and trcrgen_binout are arranged in an identical order. Therefore, the trhist can be obtained from the trcgen_binout file by using the l2a program located at http://ftp.lstc.com/- user/lsda. . The keyword *DEFINE provides a way of defining boxes, coordinate systems, load curves, tables, and orientation vectors for various uses. The keyword cards in this section are defined in alphabetical order: *DEFINE_ADAPTIVE_SOLID_TO_DES *DEFINE_ADAPTIVE_SOLID_TO_SPH *DEFINE_BOX *DEFINE_BOX_ADAPTIVE *DEFINE_BOX_COARSEN *DEFINE_BOX_DRAWBEAD *DEFINE_BOX_SPH *DEFINE_CONNECTION_PROPERTIES_{OPTION} *DEFINE_CONSTRUCTION_STAGES *DEFINE_CONTACT_EXCLUSION *DEFINE_CONTACT_VOLUME *DEFINE_COORDINATE_NODES *DEFINE_COORDINATE_SYSTEM *DEFINE_COORDINATE_VECTOR *DEFINE_CPM_BAG_INTERACTION *DEFINE_CPM_CHAMBER *DEFINE_CPM_GAS_PROPERTIES *DEFINE_CPM_VENT *DEFINE_CRASHFRONT *DEFINE_CURVE_{OPTION} *DEFINE_CURVE_BOX_ADAPTIVITY *DEFINE_CURVE_DRAWBEAD *DEFINE_CURVE_DUPLICATE *DEFINE_CURVE_ENTITY *DEFINE_CURVE_FEEDBACK *DEFINE_CURVE_FLC *DEFINE_CURVE_FUNCTION *DEFINE_CURVE_SMOOTH *DEFINE_CURVE_TRIM_{OPTION} *DEFINE_DEATH_TIMES_{OPTION} *DEFINE_DE_ACTIVE_REGION *DEFINE_DE_BOND *DEFINE_DE_BY_PART *DEFINE_DE_HBOND *DEFINE_DE_INJECTION *DEFINE_DE_MASSFLOW_PLANE *DEFINE_DE_TO_BEAM_COUPLING *DEFINE_DE_TO_SURFACE_COUPLING *DEFINE_DE_TO_SURFACE_TIED *DEFINE_ELEMENT_DEATH_{OPTION} *DEFINE_ELEMENT_GENERALIZED_SHELL *DEFINE_ELEMENT_GENERALIZED_SOLID *DEFINE_FABRIC_ASSEMBLIES *DEFINE_FILTER *DEFINE_FORMING_BLANKMESH *DEFINE_FORMING_CLAMP *DEFINE_FRICTION *DEFINE_FRICTION_ORIENTATION *DEFINE_FUNCTION *DEFINE_FUNCTION_TABULATED *DEFINE_GROUND_MOTION *DEFINE_HAZ_PROPERTIES *DEFINE_HAZ_TAILOR_WELDED_BLANK *DEFINE_HEX_SPOTWELD_ASSEMBLY_{OPTION} *DEFINE_LANCE_SEED_POINT_COORDINATES *DEFINE_MATERIAL_HISTORIES *DEFINE_MULTI_DRAWBEADS_IGES *DEFINE_PBLAST_AIRGEO *DEFINE_PBLAST_GEOMETRY *DEFINE_PLANE *DEFINE_POROUS_{OPTION} *DEFINE_PRESSURE_TUBE *DEFINE_REGION *DEFINE_SD_ORIENTATION *DEFINE_SET_ADAPTIVE *DEFINE_SPH_ACTIVE_REGION *DEFINE_SPH_DE_COUPLING *DEFINE_SPH_INJECTION *DEFINE_SPH_TO_SPH_COUPLING *DEFINE_SPOTWELD_FAILURE_{OPTION} *DEFINE_SPOTWELD_FAILURE_RESULTANTS *DEFINE_SPOTWELD_RUPTURE_PARAMETER *DEFINE_SPOTWELD_RUPTURE_STRESS *DEFINE_STAGED_CONSTRUCTION_PART *DEFINE_TABLE *DEFINE_TABLE_2D *DEFINE_TABLE_3D *DEFINE_TABLE_MATRIX *DEFINE_TARGET_BOUNDARY *DEFINE_TRACER_PARTICLES_2D *DEFINE_TRANSFORMATION *DEFINE_TRIM_SEED_POINT_COORDINATES *DEFINE_VECTOR *DEFINE_VECTOR_NODES Unless noted otherwise, an additional option “TITLE” may be appended to the *DEFINE keywords. If this option is used then an addition line is read for each section in 80a format which can be used to describe the defined curve, table, etc. At present LS- DYNA does make use of the title. Inclusion of titles gives greater clarity to input decks. Examples for the *DEFINE keyword can be found at the end of this section. *DEFINE_ADAPTIVE_SOLID_TO_DES_{OPTION} Purpose: Adaptively transform a Lagrangian solid part or part set to DES (Discrete Element Sphere) particles (elements) when the Lagrangian solid elements comprising those parts fail. One or more DES particles will be generated for each failed element as debris. The DES particles replacing the failed element inherit the properties of the failed solid element including mass, and kinematical state. The available options include: <BLANK> ID ID Card. Additional card for the ID keyword option. Optional 1 2 3 4 5 6 7 8 Variable DID Type I Default none HEADING A70 None Card 1 1 2 3 4 5 6 7 8 Variable IPID ITYPE NQ IPDES ISDES RSF OUTDES Type I I I I I F Default none none None none None 1.0 I 0 VARIABLE DESCRIPTION DID Definition ID. This must be a unique number. HEADING Definition descriptor. It is suggested that unique descriptions be used. IPID ID of the solid part or part set to transform. Figure 15-1. Left to right, illustration of conversion from solid to DES for NQ = 2 of hexahedron, pentahedron, and tetrahedron elements. VARIABLE DESCRIPTION ITYPE IPID type: EQ.0: Part ID, NE.1: Part set ID. NQ Adaptive option for hexahedral elements. For tetrahedral and pentahedral elements, see Remark 1: EQ.1: Adapt one solid element to one discrete element, EQ.2: Adapt one solid element to 8 discrete elements, EQ.3: Adapt one solid element to 27 discrete elements. IPDES ISDES Part ID for newly generated discrete elements, See Remark 2. Section ID for discrete elements, See Remark 2. RSF DES radius scale down factor. OUTDES Allow user output generated discrete element nodes and DES properties toa keyword file. EQ.0: No output. (Default) EQ.1: Write data under filename, desvfill.inc Remarks: 1. DES Element to Sold Element Ratio. The DES particles are evenly distribut- ed within the solid element. For hexahedral elements the number of the gener- ated DES particles is NQ × NQ × NQ. For pentahedral elements, the number of generated DES particles is 1, 6, and 18 for NQ = 1, 2, and 3 respectively. For tetrahedral elements, the number generated DES particles is 1, 4, and 10 for NQ = 1, 2, and 3 respectively. See Figure 15-1. 2. Part ID. The Part ID for newly generated DES particles can be either a new Part ID or the ID of an existing DES Part. *DEFINE_ADAPTIVE_SOLID_TO_SPH_{OPTION} Purpose: Adaptively transform a Lagrangian solid Part or Part Set to SPH particles, when the Lagrangian solid elements comprising those parts fail. One or more SPH particles (elements) will be generated for each failed element. The SPH particles replacing the failed solid Lagrangian elements inherit all the Lagrange nodal quantities and all the Lagrange integration point quantities of these failed solid elements. Those properties are assigned to the newly activated SPH particles. The constitutive properties assigned to the new SPH part will correspond to the MID and EOSID referenced by the SPH *PART definition. The available options include: <BLANK> ID ID Card. Additional card for the ID keyword option. Optional 1 2 3 4 5 6 7 8 Variable DID Type I Default none HEADING A70 none Card 1 1 2 3 4 5 6 7 8 Variable IPID ITYPE NQ IPSPH ISSPH ICPL IOPT CPCD Type I I I I I I I F Default none none none none none none none average VARIABLE DESCRIPTION DID Definition ID. This must be a unique number. HEADING Definition descriptor. It is suggested that unique descriptions be used. VARIABLE DESCRIPTION IPID ID of the solid part or part set to transform. ITYPE IPID type: EQ.0: Part ID, NE.0: Part set ID. NQ Adaptive option for hexahedral elements. For tetrahedral and pentahedral elements, see remark 1: EQ.n: Adapt one 8-node solid element to (𝑛 × 𝑛 × 𝑛) SPH elements. The range of n is from 1 to 8. IPSPH Part ID for newly generated SPH elements, See Remark 2. ISSPH Section ID for SPH elements, See Remark 2. ICPL Coupling of newly generated SPH elements to the adjacent solid elements: EQ.0: Failure without coupling (debris simulation), EQ.1: Coupled to Solid element. EQ.3: Pure thermal coupling between SPH part and Solid part (combined with IOPT = 0 option, See Remark 4). IOPT Coupling method (for ICPL = 1 only See Remark 3): EQ.0: Coupling from beginning (used as constraint between SPH elements and Solid elements), EQ.1: Coupling begins when Lagrange element fails. CPCD Thermal coupling conductivity between SPH part and Solid part for ICPL = 3 option. The default value is set as the average value of the conductivity from SPH part and the conductivity from Solid part. Remarks: 1. The SPH particles are evenly distributed within the solid element. For hexahedral elements the number of the generated SPH particles is NQ*NQ*NQ. For pentahedral elements, the number of generated SPH particles is 1, 6, and 18 for NQ = 1, 2, and 3 respectively. For tetrahedral elements, the number gener- ated SPH particles is 1, 4, and 10 for NQ = 1, 2, and 3 respectively. 2. The Part ID for newly generated SPH particles can be either a new Part ID or the ID of an existing SPH Part. For constraint coupling (i.e. ICPL = 1 and IOPT = 0), the newly generated SPH part ID should be different from the exist- ing one. 3. 4. ICPL = 0 is used for debris simulation, no coupling happens between newly generated SPH particles and solid elements, the user needs to define node to surface contact for the interaction between those two parts. When ICPL = 1 and IOPT = 1, the newly generated SPH particles are bonded with solid elements as one part through the coupling, and the new material ID with different failure criteria can be applied to the newly generated SPH particles. ICPL = 3 (combined with IOPT = 0) is used for pure thermal coupling between SPH part and Solid part only. User can define the coupling thermal conductivi- ty value between SPH part and Solid part through CPCD parameter for more realistic thermal coupling between SPH part and Solid part. SPH node Example of SPH nodes for hexahedron element with NQ = 2 Example of SPH nodes for pentahedron element with NQ = 2 Example of SPH nodes tetrahedron element with NQ = 2 for a Available options include: <BLANK> LOCAL *DEFINE_BOX Purpose: Define a box-shaped volume. Two diagonally opposite corner points of a box are specified in global or local coordinates if the LOCAL option is active. The box volume is then used for various specifications for a variety of input options, e.g., velocities, contact, etc. If the option, LOCAL, is active, a local coordinate system with two vectors, see Figure 15-7, is defined. The vector cross product, 𝑧 = 𝑥 × 𝑦, determines the local z-axis. The local y-axis is then given by 𝑦 = 𝑧 × 𝑥. A point, X in the global coordinate system is considered to lie with the volume of the box if the coordinate X - C, where C is the global coordinate offset vector defined on Card 3, lies within the box after transfor- mation into the local system, XC_local = T × ( X – C ). The local coordinate, XC_local, is checked against the minimum and maximum coordinates defined on Card 1 in the local system. For the *INCLUDE_TRANSFORM options that include translations and rotations, all box options are automatically converted from *DEFINE_BOX_xxxx to *DE- FINE_BOX_xxxx_LOCAL in the DYNA.INC file. Here, xxxx represents the box options: ADAPTIVE, COARSEN, and SPH, which are defined below. Card 1 2 3 4 5 6 7 8 Variable BOXID XMN XMX YMN YMX ZMN ZMX Type Default I 0 F F F F F F 0.0 0.0 0.0 0.0 0.0 0.0 8 *DEFINE_BOX Local Card 1. First additional card for LOCAL keyword option. Card 2 Variable 1 XX Type F 2 YX F 3 ZX F 4 XV F 5 YV F 6 ZV F Default 0.0 0.0 0.0 0.0 0.0 0.0 Local Card 2. Second additional card for LOCAL keyword option. 4 5 6 7 8 Card 3 Variable 1 CX Type F 2 CY F 3 CZ F Default 0.0 0.0 0.0 VARIABLE DESCRIPTION BOXID Box ID. Define unique numbers. XMN XMX YMN YMX ZMN ZMX Minimum x-coordinate. Define in the local coordinate system if the option LOCAL is active. Maximum x-coordinate. . Define in the local coordinate system if the option LOCAL is active. Minimum y-coordinate. . Define in the local coordinate system if the option LOCAL is active. Maximum y-coordinate. . Define in the local coordinate system if the option LOCAL is active. Minimum z-coordinate. . Define in the local coordinate system if the option LOCAL is active. Maximum z-coordinate. . Define in the local coordinate system if the option LOCAL is active. XX YX ZX XV YV ZV CX CY CZ *DEFINE_BOX DESCRIPTION X-coordinate on local x-axis. Origin lies at (0,0,0). Define if the LOCAL option is active. Y-coordinate on local x-axis. Define if the LOCAL option is active. Z-coordinate on local x-axis. Define if the LOCAL option is active. X-coordinate of local x-y vector. Define if the LOCAL option is active. Y-coordinate of local x-y vector. Define if the LOCAL option is active. Z-coordinate of local x-y vector. Define if the LOCAL option is active. X-global coordinate of offset vector to origin of local system. Define if the LOCAL option is active. Y-global coordinate of offset vector to origin of local system. Define if the LOCAL option is active. Z-global coordinate of offset vector to origin of local system. Define if the LOCAL option is active. Available options include: <BLANK> LOCAL *DEFINE Purpose: Define a box-shaped volume enclosing (1) the shells where the h-adaptive level (2) the solids where the tetrahedron r-adaptive mesh size is to be specified. If the midpoint of the element falls within the box, the h-adaptive level is reset. With the additions of LIDX/NDID, LIDY and LIDZ, the box can be made movable; it is also possible to define a fission box followed by a fusion box and the mesh could refine when deformed and coarsen when flattened. Shells falling outside of this volume use the value, MAXLVL, on the *CONTROL_ADAPTIVE control cards. Another related keyword includes: *DEFINE_CURVE_BOX_ADAPTIVITY. Card 1 1 2 3 4 5 6 7 8 Variable BOXID XMN XMX YMN YMX ZMN ZMX Type I F F F F F F Default none 0.0 0.0 0.0 0.0 0.0 0.0 Card 2 1 2 3 4 5 6 7 8 Variable PID LEVEL LIDX/NDID LIDY LIDZ BRMIN BRMAX Type Default I 0 I 1 I 0 I 0 I 0 F F 0.0 0.0 Local Card 1. First additional card for LOCAL keyword option. See *DEFINE_BOX for a description of the LOCAL option. Card 3 Variable 1 XX Type F 2 YX F 3 ZX F 4 XV F 5 YV F 6 ZV F 7 8 Default 0.0 0.0 0.0 0.0 0.0 0.0 Local Card 2. Second additional card for LOCAL keyword option. 4 5 6 7 8 Card 4 Variable 1 CX Type F 2 CY F 3 CZ F Default 0.0 0.0 0.0 VARIABLE DESCRIPTION BOXID Box ID. Define unique numbers. XMN XMX YMN YMX ZMN ZMX Minimum x-coordinate. Define in the local coordinate system if the option LOCAL is active. Maximum x-coordinate. Define in the local coordinate system if the option LOCAL is active. Minimum y-coordinate. Define in the local coordinate system if the option LOCAL is active. Maximum y-coordinate. Define in the local coordinate system if the option LOCAL is active. Minimum z-coordinate. Define in the local coordinate system if the option LOCAL is active. Maximum z-coordinate. Define in the local coordinate system if the option LOCAL is active. VARIABLE DESCRIPTION PID LEVEL Deformable part ID. If zero, all active elements within box are considered. Maximum number of refinement levels for elements that are contained in the box. Values of 1, 2, 3, 4,... allow a maximum of 1, 4, 16, 64, ... elements, respectively, to be created for each original element. LIDX/NDID Load curve ID/Node ID. GT.0: load curve ID. Define adaptive box movement (displacement vs. time) in global X axis. LT.0: absolute value is a node ID, whose movement will be followed by the moving adaptive box. The node ID can be on a moving rigid body. EQ.0: no movement. LIDY Load curve ID. GT.0: load curve ID. Define adaptive box movement (displacement vs. time) in global Y axis. EQ.0: no movement. LIDZ Load curve ID. GT.0: load curve ID. Define adaptive box movement (displacement vs. time) in global Z axis. EQ.0: no movement. BRMIN Minimum mesh size in 3D tetrahedron adaptivity BRMAX Maximum mesh size in 3D tetrahedron adaptivity XX YX ZX XV X-coordinate on local x-axis. Origin lies at (0,0,0). Define if the LOCAL option is active. Y-coordinate on local x-axis. Define if the LOCAL option is active. Z-coordinate on local x-axis. Define if the LOCAL option is active. X-coordinate of local x-y vector. Define if the LOCAL option is active. *DEFINE_BOX_ADAPTIVE DESCRIPTION Y-coordinate of local x-y vector. Define if the LOCAL option is active. Z-coordinate of local x-y vector. Define if the LOCAL option is active. X-global coordinate of offset vector to origin of local system. Define if the LOCAL option is active. Y-global coordinate of offset vector to origin of local system. Define if the LOCAL option is active. Z-global coordinate of offset vector to origin of local system. Define if the LOCAL option is active. YV ZV CX CY CZ Remarks: The moving adaptive box is very useful and efficient in situation where deformation progresses while happening only locally, such as roller hemming and incremental forming simulation. With the moving box feature, elements entering one box can be refined and fused together when they enter another box. Mesh fission outside of the moving box envelope is controlled by MAXLVL and other parameters under *CONTROL_ADAPTIVE. The fusion controls (NCFREQ, IADPCL) can be defined using *CONTROL_ADAPTIVE. Currently, only IADPCL = 1 is supported. Only when one of the LCIDX/NDID, LICDY, or LCIDZ is defined, the adaptive box will be moving; otherwise it will be stationary. For 3D tetrahedron r-adaptivity, the current implementation does not support LOCAL option. In card 2, PID, BRMIN and BRMAX are the only parameters currently supported in 3D r-adaptivity. Example: Referring to a partial input deck below, and Figure 15-2, a strip of sheet metal is being roller hemmed. The process consists of pre- and final hemming. Each pre- and final roller is defined with a moving adaptive box ID 2 and 3, respectively, with the box shapes shown in Figure 15-2. The first box, a fission box, was set at LEVEL = 3, while the second box, a fusion box, was set at LEVEL = 1. Elements outside of the volume envelope made by the moving boxes undergo no fission and fusion (MAXLVL = 1). This settings allows mesh fission when entering the moving box 2 (LEVEL = 3), fusion only when elements entering the moving box 3 (LEVEL = 1), no fusion/fusion (MAXLVL = 1) at all outside of the volume envelope created by the moving boxes. In the example, the boxes 2 and 3 are to be moved in global X direction for a distance of 398mm defined by load curve 11, and 450mm defined by load curve 12, respectively. *CONTROL_TERMINATION 0.252 *CONTROL_ADAPTIVE $ ADPFREQ ADPTOL ADPOPT MAXLVL TBIRTH TDEATH LCADP IOFLAG 8.05E-4 0.200000 2 1 0.0001.0000E+20 0 1 $ ADPSIZE ADPASS IREFLG ADPENE ADPTH MEMORY ORIENT MAXEL 0.300000 1 0 5.0 $ IADPN90 NCFREQ IADPCL ADPCTL CBIRTH CDEATH -1 0 1 1 10.0 0.000 10.30 *DEFINE_BOX_ADAPTIVE $# BOXID XMN XMX YMN YMX ZMN ZMX 2 -10.00000 36.000000 -15.03000 3.991000 1.00E+00 48.758000 $# PID LEVEL LIDX/NDID LIDY LIDZ 6 3 11 *DEFINE_BOX_ADAPTIVE $# BOXID XMN XMX YMN YMX ZMN ZMX 3 -100.0000 -60.0000 -15.03000 3.991000 1.00E+00 48.758000 $# PID LEVEL LIDX/NDID LIDY LIDZ 6 1 12 *DEFINE_CURVE 11 0.000 0.0 0.00100000 1.0 0.19900000 397.0 0.20000000 398.0 1.000 398.0 ⋮ ⋮ *DEFINE_CURVE 12 0.0 0.0 0.05 0.0 0.051 1.0 0.251 401.0 0.252 450.0 ⋮ ⋮ A moving box can also follow the movement of a node, which can be on a moving rigid body. In this case, load curves defining the boxes’ movement can be skipped, instead, NDIDs for the boxes should be defined. For example, in Figure 15-2 and a partial keyword example below, box 2 is to follow a node (ID: 33865) on the pre-roller, and box 3 to follow another node (ID: 38265) on the final roller. *DEFINE_BOX_ADAPTIVE $# BOXID XMN XMX YMN YMX ZMN ZMX 2 -10.00000 36.000000 -15.03000 3.991000 1.00E+00 48.758000 $# PID LEVEL LIDX/NDID LIDY LID 6 3 -33865 *DEFINE_BOX_ADAPTIVE $# BOXID XMN XMX YMN YMX ZMN ZMX 3 -100.0000 -60.0000 -15.03000 3.991000 1.00E+00 48.758000 $# PID LEVEL LIDX/NDID LIDY LID 6 3 -38265 *DEFINE_BOX_ADAPTIVE The variables LIDX/NDID, LIDY, LIDZ are available in both SMP and MPP starting in Revision 98718. Fission box: LEVEL=3, follows Node 38265 Node 33865 Inner part Outer flange Hem bed Roller path Pre-roller Node 38265 Final roller Fusion box 3: LEVEL=1, follows Node 33865 Hem bed Mesh fissioned after pre-rollers' passing Mesh fuzed after all rollers' passing Inner part Original mesh Roller path Outer flange Figure 15-2. Defining mesh fission and fusion. *DEFINE_BOX_COARSEN_{OPTION} Available options include: <BLANK> LOCAL Purpose: Define a specific box-shaped volume indicating elements which are protected from mesh coarsening. See also *CONTROL_COARSEN. Card 1 2 3 4 5 6 7 8 Variable BOXID XMN XMX YMN YMX ZMN ZMX IFLAG Type I F F F F F F Default none 0.0 0.0 0.0 0.0 0.0 0.0 I 0 Local Card 1. First additional card for LOCAL keyword option. See *DEFINE_BOX for a description of the LOCAL option. Card 2 Variable 1 XX Type F 2 YX F 3 ZX F 4 XV F 5 YV F 6 ZV F 7 8 Default 0.0 0.0 0.0 0.0 0.0 0.0 Local Card 2. Second additional card for LOCAL keyword option. 4 5 6 7 8 Card 3 Variable 1 CX Type F 2 CY F 3 CZ F Default 0.0 0.0 0.0 VARIABLE DESCRIPTION BOXID Box ID. Define unique numbers. XMN XMX YMN YMX ZMN ZMX Minimum x-coordinate. Define in the local coordinate system if the option LOCAL is active. Maximum x-coordinate. . Define in the local coordinate system if the option LOCAL is active. Minimum y-coordinate. . Define in the local coordinate system if the option LOCAL is active. Maximum y-coordinate. . Define in the local coordinate system if the option LOCAL is active. Minimum z-coordinate. . Define in the local coordinate system if the option LOCAL is active. Maximum z-coordinate. . Define in the local coordinate system if the option LOCAL is active. IFLAG Flag for protecting elements inside or outside of box. EQ.0: elements inside the box cannot be coarsened EQ.1: elements outside the box cannot be coarsened XX YX ZX XV YV ZV CX X-coordinate on local x-axis. Origin lies at (0,0,0). Define if the LOCAL option is active. Y-coordinate on local x-axis. Define if the LOCAL option is active. Z-coordinate on local x-axis. Define if the LOCAL option is active. X-coordinate of local x-y vector. Define if the LOCAL option is active. Y-coordinate of local x-y vector. Define if the LOCAL option is active. Z-coordinate of local x-y vector. Define if the LOCAL option is active. X-global coordinate of offset vector to origin of local system. Define if the LOCAL option is active. Y-global coordinate of offset vector to origin of local system. Define if the LOCAL option is active. Z-global coordinate of offset vector to origin of local system. Define if the LOCAL option is active. *DEFINE VARIABLE CY CZ Remarks: 1. Many boxes may be defined. If an element is protected by any box then it may not be coarsened. *DEFINE Purpose: Define a specific box or tube shaped volume around a draw bead. This option is useful for the draw bead contact. If box shaped, the volume will contain the draw bead nodes and elements between the bead and the outer edge of the blank. If tubular, the tube is centered around the draw bead. All elements within the tubular volume are included in the contact definition. Card 1 2 3 4 5 6 7 8 Variable BOXID PID SID IDIR STYPE RADIUS CID Type Default I 0 F F F 0.0 0.0 0.0 I 4 F 0.0 I 0 Remarks optional optional VARIABLE DESCRIPTION BOXID Box ID. Define unique numbers. PID SID IDIR Part ID of blank. Set ID that defines the nodal points that lie along the draw bead. If a node set is defined, the nodes in the set must be consecutive along the draw bead. If a part or part set is defined, the set must consist of beam or truss elements. Within the part set, no ordering of the elements is assumed, but the number of nodes must equal the number of beam elements plus 1. Direction of tooling movement. The movement is in the global coordinate direction unless the tubular box option is active and CID is nonzero. In this latter case, the movement is in the local coordinate direction. EQ.1: tooling moves in x-direction, EQ.2: tooling moves in y-direction, EQ.3: tooling moves in z-direction. STYPE Set type: *DEFINE_BOX_DRAWBEAD DESCRIPTION EQ.2: part set ID, EQ.3: part ID, EQ.4: node set ID. RADIUS The radius of the tube, which is centered around the draw bead. Elements of part ID, PID, that lie within the tube will be included in the contact. If the radius is not defined, a rectangular box is used instead. This option is recommended for curved draw beads and for draw beads that are not aligned with the global axes. CID Optional coordinate system ID. This option is only available for the tubular drawbead. Available options include: <BLANK> LOCAL *DEFINE Purpose: Define a box-shaped volume. Two diagonally opposite corner points of a box are specified in global coordinates. Particle approximations of SPH elements are computed when particles are located inside the box. The load curve describes the motion of the maximum and minimum coordinates of the box. Card 1 1 2 3 4 5 6 7 8 Variable BOXID XMN XMX YMN YMX ZMN ZMX VID Type I F F F F F F Default none 0.0 0.0 0.0 0.0 0.0 0.0 4 5 6 7 Card 2 1 Variable LCID Type Default I 0 2 VD I 0 3 NID I 0 I 0 Local Card 1. First additional card for LOCAL keyword option. See *DEFINE_BOX for a description of the LOCAL option Card 3 Variable 1 XX Type F 2 YX F 3 ZX F 4 XV F 5 YV F 6 ZV F 7 8 Default 0.0 0.0 0.0 0.0 0.0 0.0 Local Card 2. Second additional card for LOCAL keyword option. 4 5 6 7 8 Card 4 Variable 1 CX Type F 2 CY F 3 CZ F Default 0.0 0.0 0.0 VARIABLE DESCRIPTION BOXID Box ID. Define unique numbers. XMN XMX YMN YMX ZMN ZMX Minimum x-coordinate. Define in the local coordinate system if the option LOCAL is active. Maximum x-coordinate. Define in the local coordinate system if the option LOCAL is active. Minimum y-coordinate. Define in the local coordinate system if the option LOCAL is active. Maximum y-coordinate. Define in the local coordinate system if the option LOCAL is active. Minimum z-coordinate. Define in the local coordinate system if the option LOCAL is active. Maximum z-coordinate. Define in the local coordinate system if the option LOCAL is active. VARIABLE DESCRIPTION VID LCID Vector ID for DOF, see *DEFINE_VECTOR. Load curve ID to describe motion value versus time, see *DE- FINE_CURVE VD Velocity/Displacement flag: EQ.0: velocity, EQ.1: displacement, EQ.2: referential node NID Referential nodal ID for VD = 2 (SPH box will move with this node). XX YX ZX XV YV ZV CX CY CZ X-coordinate on local x-axis. Origin lies at (0,0,0). Define if the LOCAL option is active. Y-coordinate on local x-axis. Define if the LOCAL option is active. Z-coordinate on local x-axis. Define if the LOCAL option is active. X-coordinate of local x-y vector. Define if the LOCAL option is active. Y-coordinate of local x-y vector. Define if the LOCAL option is active. Z-coordinate of local x-y vector. Define if the LOCAL option is active. X-global coordinate of offset vector to origin of local system. Define if the LOCAL option is active. Y-global coordinate of offset vector to origin of local system. Define if the LOCAL option is active. Z-global coordinate of offset vector to origin of local system. Define if the LOCAL option is active. *DEFINE_CONNECTION_PROPERTIES_{OPTION} Available options include: <BLANK> ADD Purpose: Define failure related parameters for solid element spot weld failure by *MAT_SPOTWELD_DAIMLERCHRYSLER. For each connection identifier, CON_ID, a separate *DEFINE_CONNECTION_PROPERTIES section must be included. The ADD option allows material specific properties to be added to an existing connection ID. See Remark 2. Card 1 1 2 3 4 5 6 7 8 Variable CON_ID PRUL AREAEQ DGTYP MOARFL Type Default F 0 Card 2 1 I 0 2 I 0 3 4 I 0 5 I 0 6 7 8 Variable DSIGY DETAN DDGPR DRANK DSN DSB DSS Type F F F F F F F Default none none 1010 none none none none Card 3 1 2 3 4 5 6 7 8 Variable DEXSN DEXSB DEXSS DLCSN DLCSB DLCSS DGFAD DSCLMRR Type F F F Default 1.0 1.0 1.0 I 0 I 0 I 0 F F none 1.0 Material Specific Data: For each shell material with material specific data, define for this CON_ID the following two cards. Add as many pairs of cards as necessary. This input is terminated by the next keyword (“*”) card. Material Data Card 1. Card 4 1 2 3 4 5 Variable MID SGIY ETAN DGPR RANK Type F F F F F Default 1010 6 SN F 7 SB F 8 SS F Material Data Card 2. Card 5 1 2 3 4 5 6 7 8 Variable EXSN EXSB EXSS LCSN LCSB LCSS GFAD SCLMRR Type F F F I I I F F Default VARIABLE CON_ID 1.0 DESCRIPTION Connection ID, referenced on *MAT_SPOTWELD_DAIMLER- CHRYSLER. Multiple sets of connection data may be used by assigning different connection IDs. *DEFINE_CONNECTION_PROPERTIES DESCRIPTION PRUL The failure rule number for this connection. EQ.1: Use data of weld partner with lower RANK (default). GE.2: Use DEFINE_FUNCTION expressions to determine weld data depending on several values of both weld partners. Variables DSIGY, DETAN, DDGPR, DSN, DSB, DSS, DEXSN, DEXSB, DEXSS, and DGFAD must be defined as function IDs, see Remark 5. AREAEQ Area equation number for the connection area calculation. EQ.0: (default) Areatrue = Areamodelled EQ.1: millimeter form; see Remark 4 EQ.-1: meter form; see Remark 4 DGTYP Damage type EQ.0: EQ.1: EQ.2: no damage function is used strain based damage failure function based damage EQ.3 or 4: fading energy based damage; see Remark 4 MOARFL Modeled area flag EQ.0: Areamodelled goes down with shear (default) EQ.1: Areamodelled stays constant DSIGY Default yield stress for the spot weld element. DETAN Default tangent modulus for the spot weld element. DDGPR Default damage parameter for hyperbolic based damage function. DRANK Default rank value. DSN DSB DSS Default normal strength. Default bending strength. Default shear strength. DEXSN Default exponent on normal stress term. DEXSB Default exponent on bending stress term. VARIABLE DESCRIPTION DEXSS Default exponent on shear stress term. DLCSN DLCSB DLCSS Default curve ID for normal strength scale factor as a function of strain rate. Default curve ID for bending strength scale factor as a function of strain rate. Default curve ID for shear strength scale factor as a function of strain rate. DGFAD Default fading energy for damage type 3 and type 4. DSCLMRR Default scaling factor for torsional moment in failure function. MID SIGY ETAN DGPR Material ID of the shell material for which properties are defined. Yield stress to be used in the spot weld element calculation. Tangent modulus to be used in the spot weld element calculation. Damage parameter for hyperbolic based damage function. RANK Rank value. See Remark 4. SN SB SS EXSN EXSB EXSS LCSN LCSB LCSS Normal strength. Bending strength. Shear strength. Exponent on normal stress term. Exponent on bending stress term. Exponent on shear stress term. Curve ID for normal strength scale factor as a function of strain rate. Curve ID for bending strength scale factor as a function of strain rate. Curve ID for shear strength scale factor as a function of strain rate. *DEFINE_CONNECTION_PROPERTIES DESCRIPTION GFAD Fading energy for damage type 3 and 4. SCLMRR Scaling factor for torsional moment in failure function. Remarks: 1. Restriction to *MAT_SPOTWELD_DAIMLERCHHRYSLER. This keyword is used only with *MAT_SPOTWELD_DAIMLERCHRYSLER. The data input is used in a 3 parameter failure model. Each solid spot weld element connects shell elements that may have the same or different materials. The failure model assumes that failure of the spot weld depends on the properties of the welded materials, so this keyword allows shell material specific data to be input for the connection. The default data will be used for any spot weld connected to a shell material that does not have material specific data defined, so it is not necessary to define material specific data for all welded shell materials. 2. ADD Option. To simplify data input, the ADD keyword option allows material specific data to be added to an existing *DEFINE_CONNECTION_PROPER- TIES table. To use the ADD option, omit cards 2 and 3, and input only CON_- ID on card 1. Then use cards 4 and 5 to input material specific data. For each unique CON_ID, control parameters and default values must be input in one set of *DEFINE_CONNECTION_PROPERTIES data. The same CON_ID may be used for any number of sets of material specific data input with the ADD option. 3. The Three Parameter Failure Function. The three parameter failure function is 𝐹) 𝑓 = ( 𝜎𝑛 𝜎𝑛 𝑚𝑏 + ( 𝑚𝑛 + ( 𝜎𝑏 𝜎𝑏 where the three strength terms are SN, SB, and SS, and the three exponents are EXSN, EXSB, and EXSS. The strengths may be a function of strain rate by using the load curves, LCSN, LCSB, and LCSS. The peak stresses in the numerators are calculated from force resultants and simple beam theory. 𝜏𝐹) 𝑚𝜏 − 1 , 𝐹) 𝜎𝑛 = 𝑁𝑟𝑟 , 𝜎𝑏 = 2 + 𝑀𝑟𝑡 √𝑀𝑟𝑠 , 𝜏 = SCLMRR × 𝑀𝑟𝑟 2𝑍 + 2 + 𝑁𝑟𝑡 √𝑁𝑟𝑠 where the area is the cross section area of the weld element and Z is given by: 𝑍 = 𝜋 𝑑3 32 where d is the equivalent diameter of the solid spot weld element assuming a circular cross section. 4. Control Parameters PRUL, AREAQ. And DGTYP. There are three control parameters that define how the table data will be used for the connection, PRUL, AREAEQ, and DGTYP. PRUL determines how the parameters will be used. Because each weld connects two shell surfaces, one weld can have two sets of failure data as well as two values for ETAN and SIGY. For PRUL=1 (default), a simple rule is implemented and the data with the lower RANK will be used. For PRUL=2 or 3, function expressions can be used to determine the data based on several input values from both weld partners . The second control parameter is AREAEQ which specifies a rule for calculating a true weld cross section area, 𝐴true to be used in the failure function in place of the modeled solid element area, 𝐴. For AREAEQ = 1, 𝐴true is calculated by (5√𝑡min shell) 𝐴true = where 𝑡min shell is the thickness of the welded shell surface that has the smaller thickness. For AREAEQ = −1, 𝐴true is calculated by 𝐴true = ( 1000 √1000 × 𝑡min shell) The equation for AREAEQ = 1 is valid only for a length unit of millimeters, and AREAEQ = −1 is valid only for a length unit of meters. The third control parameter, DGTYP, chooses from two available damage types. For DGTYP = 0, damage is turned off and the weld fails immediately when 𝑓 ≥ 0. For DGTYP > 0, damage is initiated when 𝑓 ≥ 0 and complete fail- ure occurs when 𝜔 ≥ 1. For DGTYP = 1, damage growth is a function of plastic strain: 𝜔 = 𝑝 − 𝜀failure 𝜀eff − 𝜀failure 𝜀rupture , 𝜀failure ≤ 𝜀eff 𝑝 ≤ 𝜀rupture 𝑝 is the effective plastic strain in the weld material. When the value of where 𝜀eff the failure function first exceeds zero, the plastic strain at failure𝜀failure is set to the current plastic strain, and the rupture strain is offset from the plastic strain at failure by 𝜀rupture = 𝜀failure + RS − EFAIL where RS and EFAIL are the rupture strain and plastic strain at failure which are input on the *MAT_SPOTWELD_DAIMLERCHRYSLER card. If failure occurs when the plastic strain is zero, the weld material yield stress is reduced to the current effective stress such that damage can progress. For DGTYP = 2, damage is a function of the failure function, f: 𝑓 ≥ 0 ⇒ 𝜔 = 𝑓rupture where 𝑓rupture is the value of the failure function at rupture which is defined by 𝑓rupture = RS − EFAIL and RS and EFAIL are input on the *MAT_SPOTWELD_DAIMLERCHRYSLER card. Because the DGTYP = 1 damage function is scaled by plastic strain, it will mon- otonically increase in time. The DGTYP = 2 damage function is forced to be a monotonically increasing function in time by using the maximum of the current value and the maximum previous value. For both DGTYP = 1 and DGTYP = 2, the stress scale factor is then calculated by 𝜎̂ = DGPR × (1 − 𝜔) 𝜎 𝜔 (1 + √1 + DGPR) + DGPR This equation becomes nearly linear at the default value of DGPR which is 1010. For DGTYP = 3, damage is a function of total strain: 𝜔 = ∆𝜀𝑛 ∆𝜀fading where Δ𝜀𝑛 is the accumulated total strain increment between moment of dam- age initiation (failure) and current time step 𝑡𝑛 ∆𝜀𝑛 = ∆𝜀𝑛−1 + ∆𝑡𝑛√ tr(𝛆̇𝑛𝜺̇𝑛 T) , ∆𝜀|𝑡failure = 0 and 𝛥𝜀𝑓𝑎𝑑𝑖𝑛𝑔 is the total strain increment for fading (reduction of stresses to zero) ∆𝜀fading = 2 × GFAD 𝜎failure where GFAD is the fading energy from input and 𝜎failure is the effective stress at failure. The stress scale factor is then calculated by a linear equation 𝜎̂ = (1 − 𝜔)𝜎 where 𝜎 is the Cauchy stress tensor at failure and 𝜔 is the actual damage value. Problems can occur, if the loading direction changes after the onset of failure, since during the damage process, the components of the stress tensor are kept constant and hence represent the stress state at failure. Therefore DGTYP = 4 should be used describing the damage behavior of the spotweld in a more realistic way. For DGTYP = 4, damage is a function of the internal work done by the spotweld after failure, 𝜎̂ = (1 − 𝜔)𝜎 ep, 𝜔 = 𝐺used 2 × GFAD , 𝐺used = 𝐺used 𝑛−1 + det (𝐹𝑖𝑗𝜎𝑖𝑗 epΔ𝜀𝑖𝑗) Therein, 𝐹𝑖𝑗 is the deformation gradient. 𝜎 ep is a scaled Cauchy stress tensor based on the undamaged Cauchy stress tensor 𝜎 wd and scaled in such a way that the same internal work is done in the current time step as in the time step before (equipotential): 𝜎 ep = 𝛼𝜎 wd, 𝛼 = 𝑛−1,epΔ𝜀𝑖𝑗 𝜎𝑖𝑗 wdΔ𝜀𝑖𝑗 𝜎𝑖𝑗 5. Failure Rule from *DEFINE_FUNCTION. The failure rule number PRUL = 2 or 3, is available starting with Release R7. To use this new option, 11 variables have to be defined as function IDs: DSIGY, DETAN, DDGPR, DSN, DSB, DSS, DEXSN, DEXSB, DEXSS, DGFAD, and DSCLMRR. These functions depend on: (t1, t2) = thicknesses of both weld partners (sy1, sy2) = initial yield stresses at plastic strain (sm1, sm2) = maximum engineering yield stresses 𝑟 = strain rate 𝑎 = spot weld area For DSIGY = 100 Such a function could look like: *DEFINE_FUNCTION 100 func(t1,t2,sy1,sy2,sm1,sm2,r,a)=0.5*(sy1+sy2) All the listed arguments in their correct order must be included in the argument list. For PRUL = 2, the thinner part is the first weld partner. For PRUL = 3, the bottom part (nodes 1-2-3-4) is the first weld partner. Since material parameters have to be identified from both weld partners during initialization, this feature is only available for a subset of material models at the moment, namely material types 24, 120, 123, and 124. This new option eliminates the need for the ADD option. *DEFINE_CONSTRUCTION_STAGES Purpose: Define times and durations of construction stages. Card 1 2 3 4 5 6 7 8 Variable ISTAGE ATS ATE ATR RTS RTE Type I F F F F F Default none 0.0 0.0 none ATS ATE VARIABLE DESCRIPTION ISTAGE Stage ID Analysis time at start of stage Analysis time at end of stage Analysis time duration of ramp Real time at start of stage Real time at end of stage ATS ATE ATR RTS RTE Remarks: See also *CONTROL_CONSTRUCTION_STAGES and *DEFINE_STAGED_CON- STRUCTION_PART. The first stage should start at time zero. There must be no gaps between stages, i.e. ATS for each stage must be the same as ATE for the previous stage. The ramp time allows gravity loading and part stiffening/removal to be applied gradually during the first time period ATR of the construction stage. The analysis always runs in “analysis time” – typically measured in seconds. The “real time” is used only as a number to appear on output plots and graphs, and is completely arbitrary. A dynain file is written at the end of each stage. *DEFINE Purpose: Exclude tied nodes from being treated in specific contact interfaces. This keyword is currently only available in the MPP version. Card 1 1 2 3 4 5 6 7 8 Variable EID Type I Title A70 ID Card 1. This card sets the contact interface the ids of up to 7 tied interfaces. Card 2 1 Variable Target Type I 2 C1 I 3 C2 I 4 C3 I 5 C4 I 6 C5 I 7 C6 I 8 C7 I Optional ID Cards. More tied interfaces. Include as many cards as necessary. Card 2 Variable 1 C8 Type I 2 C9 I 3 4 5 6 7 8 C10 C11 C12 C13 C14 C15 I I I I I I VARIABLE DESCRIPTION EID Title Target Exclusion ID Exclusion Title Contact interface from which tied nodes are to be excluded. This must be the ID of a SINGLE_SURFACE, NODE_TO_SURFACE, or SURFACE_TO_SURFACE contact with SOFT ≠ 2. Ci *DEFINE_CONTACT_EXCLUSION DESCRIPTION The IDs of TIED contacts: 7 on the first card and 8 per additional card for as many cards as necessary. Any node which is a slave node in one of these interfaces, and is in fact tied, will not be processed (as a slave node) in the Target interface. Note that if a node is excluded from the Target by this mechanism, contact forces may still be applied to the node due to any slave or master nodes impacting the contact segments of which it is a part (no contact SEGMENTS are deleted, only contact NODES). If the Target contact is of type SURFACE_TO_SURFACE, any tied slave nodes are deleted from both the slave side (for the normal treatment) and the master side (for the symmetric treatment). *DEFINE Purpose: Define a rectangular, a cylindrical, or a spherical volume in a local coordinate system. The volume can be referenced by *SET_NODE_GENERAL for the purpose of defining a node set consisting of nodes inside the volume, or by *CONTACT_... for the purpose of defining nodes or segments on the slave side or the master side of the contact . Card 1 1 2 3 Variable CVID CID TYPE Type Default I 0 I 0 I 0 4 XC F 0. 5 YC F 0. 6 ZC F 0. 7 8 Card 2 for Rectangular Prism. Use when type = 0. Card 2 1 2 3 4 5 6 7 8 Variable XMN XMX YMN YMX ZMN ZMX Type F F F F F F Default 0.0 0.0 0.0 0.0 0.0 0.0 Card 2 for Cylinder. Use when type = 1. Card 2 1 2 3 4 5 6 7 8 Variable LENGTH RINNER ROUTER D_ANGC Type F F F F Default 0.0 0.0 0.0 0.0 Card 2 for Sphere Use when type = 3. Card 2 1 2 3 4 5 6 7 8 Variable RINNER ROUTER D_ANGS Type F F F Default 0.0 0.0 0.0 VARIABLE DESCRIPTION CVID CID TYPE XC YC ZC XMN XMX YMN YMX ZMN ZMX Contact volume ID Coordinate system ID. Required for rectangular and cylindrical volumes Volume type. Set to 0 for rectangular, 1 for cylindrical, and 2 for spherical. x-coordinate which defines the origin of coordinate system or the center of the sphere for type = 3 referenced to the global coordinate system. y-coordinate which defines the origin of coordinate system or the center of the sphere for type = 3 referenced to the global coordinate system. z-coordinate which defines the origin of coordinate system or the center of the sphere for type = 3 referenced to the global coordinate system. Minimum x-coordinate in local coordinate system. Maximum x-coordinate in local coordinate system. Minimum y-coordinate in local coordinate system. Maximum y-coordinate in local coordinate system. Minimum z-coordinate in local coordinate system. Maximum z-coordinate in local coordinate system. VARIABLE LENGTH DESCRIPTION Length of cylinder originating at (XC,YC,ZC) and revolving around the local x-axis. RINNER Inner radius of cylinder or sphere. ROUTER Outer radius of cylinder or sphere. D_ANGC D_ANGS If the included angle between the axis of the cylinder and the normal vector to the contact segment is less than this angle, the segment is deleted. If the included angle between a line draw from the center of the sphere to the centroid of the segment, and the normal vector to the contact segment is greater than this angle, the segment is deleted. *DEFINE_COORDINATE_NODES Purpose: Define a local coordinate system with three node numbers. The local cartesian coordinate system is defined in the following steps. If the primary direction is along the x-axis, then the 𝑧-axis is computed from the cross product of 𝑥 and 𝑦̅, , 𝑧 = 𝑥 × 𝑦̅, then the 𝑦-axis is computed via 𝑦 = 𝑧 × 𝑥. A similar procedure applies if the local axis is along the y or z axes. Card 1 Variable CID Type Default I 0 2 N1 I 0 3 N2 I 0 4 N3 I 0 5 6 7 8 FLAG DIR I 0 A X VARIABLE DESCRIPTION CID Coordinate system ID. A unique number has to be defined. N1 N2 N3 FLAG ID of node located at local origin. ID of node located along local x-axis if DIR = X, the y-axis if DIR = Y, and along the z axis if DIR = Z. ID of node located in local x-y plane if DIR = X, the local y-z plane if DIR = Y, and the local z-x plane if DIR = Z. Set to unity, 1, if the local system is to be updated each time step. Generally, this option when used with nodal SPC's is not recommended since it can cause excursions in the energy balance because the constraint forces at the node may go through a displacement if the node is partially constrained. DIR Axis defined by node N2 moving from the origin node N1. The default direction is the x-axis. Remarks: 1. The nodes N1, N2, and N3 must be separated by a reasonable distance and not colinear to avoid numerical inaccuracies. Figure 15-3. Definition of local coordinate system using three nodes when the node N2 lies along the x-axis. *DEFINE_COORDINATE_SYSTEM_{OPTION} Available options include: <BLANK> IGES Purpose: Define a local coordinate system. This card implements the same method as *DEFINE_COORDINATE_NODES; but, instead of reading coordinate positions from nodal IDs, it directly reads the three coordinates from its data cards as Cartesian triples. When the IGES option is active, LS-DYNA will generate the coordinate system from an IGES file containing three straight curves representing the x, y, and z axes. See remark 4. Card 1 for <BLANK> Keyword Option. Card 1 1 Variable CID Type Default I 0 2 XO F 3 YO F 4 ZO F 5 XL F 6 YL F 7 ZL F 0.0 0.0 0.0 0.0 0.0 0.0 8 CIDL I 0 4 5 6 7 8 Card 2 for <BLANK> Keyword Option. Card 2 Variable 1 XP Type F 2 YP F 3 ZP F Default 0.0 0.0 0.0 *DEFINE Card 1 1 2 3 4 5 6 7 8 Variable Type Default FILENAME C none VARIABLE DESCRIPTION CID Coordinate system ID. A unique number has to be defined. XO YO ZO XL YL ZL CIDL XP YP ZP X-coordinate of origin. Y-coordinate of origin. Z-coordinate of origin. X-coordinate of point on local x-axis. Y-coordinate of point on local x-axis. Z-coordinate of point on local x-axis. Coordinate system ID applied to the coordinates used to define the current system. The coordinates X0, Y0, Z0, XL, YL, ZL, XP, YP, and ZP are defined with respect to the coordinate system CIDL. X-coordinate of point in local x-y plane. Y-coordinate of point in local x-y plane. Z-coordinate of point in local x-y plane. FILENAME Name of the IGES file containing three curves . Remarks: 1. The coordinates of the points must be separated by a reasonable distance and not co-linear to avoid numerical inaccuracies. Airbag Application Boundary Constrained Contact Damping Database Define Box Coordinate Vector Elements Initial Load Rigidwall Set Data Show Cre Mod Del Global Local Label: None Coord Type *SYSTEM Position Node New ID C_Element C_Edge CID Title N+Xaxis Nodes TRAN ROTA Geopts Refl Origin X-Axis XYP Avg_Cen 3PtCircle C_Cur/Surf Geometry Compute X: Y: Z: Origin XYPlane Clear AlongX AlongY AlongZ Apply Done Cancel NID Create Create Position All None Rev AList Apply Cancel Write Done Create Entity Figure 15-4. LS-PrePost4.0 Dialog for defining a coordinate system. 2. Care must be taken to avoid chains of coordinate transformations because there is no guarantee that they will be executed in the correct order. 3. LS-PrePost. A coordinate system can be created using the dialog box located at Model (main window) → CreEnt → Define → Coordinate. This will activate a Define Coordinate dialog in the right pane. Select the Cre radio button at the top of the right pane, and set the type dropdown to *SYSTEM. The next set of radio buttons (below the title input box) sets the method used to define the coordinate system. See Figure 15-4. a) The N+Xaxis method generates a coordinate system from based on: i) ii) a user specified origin, one of the three global axes (this is a severe restriction), and iii) a 3rd point. N+Xaxis Nodes TRAN ROTA Geopts Refl Origin X-Axis XYP Origin X-Axis XYPlane Direction X Clear Figure 15-5. Subset of Create Entity dialog for both Nodes and Geopts methods. The 3rd point, together with the specified global axis defines the new sys- tem’s x-y plane. The remaining axes are derived using orthogonality and right-handedness. This method requires the user to pick two points which involves the Create Position dialog box, as shown in the left frame of Figure 15-4. NOTE: After defining each point in the Create Position dialog, it is very important to use the done button. The Create Entity dialog stays up and remains interactive while the Create Position dialog is also up and interactive. This can be confusing. Returning to the Cre- ate Entity dialog without choosing done is a common mistake. b) The node method generates a coordinate system from three points: i) The first point specifies the origin. ii) The first and second points together specify the x-axis. iii) The three points together specify the x-y plane of the new coordi- nate system. The y and z axis are derived from orthogonality and right-handedness. c) The Geopts option generates the new coordinate system from a global axis and two points. With this method the new system’s z-axis is set from the Direction drop-down. This new system’s x-y plane is, then, orthogonal to the chosen direction. The remaining two points serve to define the origin and the x-axis (by projecting the second point). This option is useful for metal forming application, since, often times, only the z-axis is important while the while the x and y axes are not. Longest length curve Local Z-axis Mid-length curve Local Y-axis B3 B2 B1 Shortest length curve Local X-axis Figure 15-6. Input curves (left). The generated local coordinate system is written to the d3plot file as a part consisting of three beams (right). 4. IGES. When option, IGES, is used, three curves in the IGES format will be used to define a local coordinate system. IGES curve entity types 126, 110 and 106 are currently supported. Among the three curves, the longest length will be made as local Z-axis, the mid-length will be Y-axis and the shortest length X- axis. Suggested X, Y and Z-axis length is 100mm, 200mm and 300mm, respec- tively. All the three curves must have one identical point, and will be used for the origin of the new local coordinate system. The coordinate system ID for the local system will be based on the IGES file name. The IGES file name must start with a number, followed by an underscore “_”, or by a dot. The number pre- ceding the file name will be used as the new local coordinate system ID, which can then be referenced in *MAT_20 cards, for example. After the LS-DYNA run, three beam elements of a new PID will be created in place of the three curves representing the local X, Y, and Z-axis in the d3plot file for viewing in LS-PrePost. See Figure 15-6. The following partial input contains an example in which the keyword is used to create a local coordinate system (CID = 25) from IGES input. The IGES file named, 25_iges, contains three intersecting curves in one of the three supported IGES entity types. The example demonstrates using the IGES coordinate sys- tem (ID = 25) to specify the local coordinate system for a rigid body (PID = 2, MID = 2). The keyword, *BOUNDARY_PRESCRIBED_MOTION_RIGID_ LO- CAL, then uses this local coordinate system to assign velocities from load curves 3 and 5 for the rigid body motion in the local x-direction. *KEYWORD *DEFINE_COORDINATE_SYSTEM_IGES_TITLE Flanging OP25 25_iges $---+----1----+----2----+----3----+----4----+----5----+----6----+----7----+--- -8 *PART punch 2 2 2 *MAT_RIGID $ MID RO E PR N COUPLE M ALIAS 2 7.830E-09 2.070E+05 0.28 $ CMO CON1 CON2 -1 25 011111 $LCO or A1 A2 A3 V1 V2 V3 25 $---+----1----+----2----+----3----+----4----+----5----+----6----+----7----+--- -8 *BOUNDARY_PRESCRIBED_MOTION_RIGID_LOCAL $ typeID DOF VAD LCID SF VID DEATH BIRTH 2 1 0 3 -1.0 0 0.00241 0.0 2 1 0 5 -1.0 0 0.0115243 0.00241 The keyword can be repeated for each new coordinate system if multiple coor- dinate systems are needed. Revision information: This option is available starting in LS-DYNA Revision 62798. *DEFINE_COORDINATE_VECTOR Purpose: Define a local coordinate system with two vectors, see Figure 15-7. The vector cross product, 𝑧 = 𝑥 × 𝑥𝑦, determines the z-axis. The y-axis is then given by 𝑦 = 𝑧 × 𝑥. If this coordinate system is assigned to a nodal point, then at each time step during the calculation, the coordinate system is incrementally rotated using the angular velocity of the nodal point to which it is assigned. Card 1 Variable CID Type Default I 0 2 XX F 3 YX F 4 ZX F 5 XV F 6 YV F 7 ZV F 8 NID I 0.0 0.0 0.0 0.0 0.0 0.0 0. VARIABLE DESCRIPTION CID Coordinate system ID. A unique number has to be defined. X-coordinate on local x-axis. Origin lies at (0,0,0). Y-coordinate on local x-axis Z-coordinate on local x-axis X-coordinate of local x-y vector Y-coordinate of local x-y vector Z-coordinate of local x-y vector Optional nodal point ID. The coordinate system rotates with the rotation of this node. If the node is not defined, the coordinate system is stationary. XX YX ZX XV YV ZV NID Remarks: 1. These vectors should be separated by a reasonable included angle to avoid numerical inaccuracies. 2. Ideally, this nodal point should be attached to a rigid body or a structural part where the nodal point angular velocities are meaningful. It should be noted that angular velocities of nodes may not be meaningful if the nodal point is attached only to solid elements and even to shell elements where the drilling degree of freedom may be singular, which is likely in flat geometries. xy y x Figure 15-7. Definition of the coordinate system with two vectors. Origin (0,0,0) *DEFINE_CPM_BAG_INTERACTION Purpose: To model energy flow from a master airbag to a slave airbag. The master must be an active particle airbag and the slave a control volume (CV) airbag converted from a particle bag. To track the flow of energy, LS-DYNA automatically determines which vent parts are common to both airbags. At each time step the energy that is vented through the common vents is subtracted from the master and added to the slave. In turn, the slave bag’s pressure provides the downstream pressure value for the master bag’s venting equation. While this model accounts for energy flow from master to slave it ignores flow from slave to master. If CHAMBER is used for slave CV bag, see remark 1. Card 1 1 2 3 4 5 6 7 8 Variable Bag ID1 Bag ID2 Type I I Default none none VARIABLE DESCRIPTION Airbag ID of master CPM particle bag Airbag ID of slave CV bag switched from CPM bag Bag ID1 Bag ID2 Remarks: 1. Due to the complexity of the bookkeeping, the slave may have several chambers but only one of the chambers is allowed to interact with the master bag. This chamber will be searched automatically through the commonly shared parts. *DEFINE Purpose: To define airbag chambers for air particle initialization or chamber interaction. Card 1 Variable 1 ID Type I Default none 2 3 4 5 6 7 8 NCHM I 0 Chamber Definition Card Sets: Add NCHM chamber definition card sets. Each chamber definition card set consists of a Chamber Definition Card followed by NINTER Interaction Cards. Chamber Definition Card. Card 2 1 2 3 4 5 6 7 8 Variable SID1 SID2 NINTER CHM_ID Type I Default none I 0 I 0 I 0 Interaction Cards. Add NINTER of these. If NINTER = 0, skip this card. Card 3 1 2 3 4 5 6 7 8 Variable SID3 ITYPE3 TOCHM Type I I I Default none none none P3 P1 Chamber 997 Chamber 998 P2 P4 Figure 15-8. VARIABLE DESCRIPTION ID Unique ID for this card NCHM Number of chambers defined in this card SID1 SID2 Part set defining all parts that constitute the chamber volume Part set defining the parts whose shell normals need to be flipped (eg. separation walls between chambers) NINTER Number of vent hole definition for chamber interaction. CHM_ID Chamber ID . SID3 Set defining interaction between chambers ITYPE3 Set type EQ.0: Part EQ.1: Part set TOCHM The chamber ID of the connected chamber. *DEFINE 1. Each chamber's volume is calculated based on the part normals pointed inwards. So SID1 would normally have parts with their shell normals pointing inwards. But in some cases, parts may be shared by more than one chamber. In this case, the shell orientation of certain part(s) may need to be flipped for the other chambers in question. In such cases, SID2 can be used to flip the shell- normals for specific parts. *SET_PART_LIST $# sid 1 $# pid1 pid2 pid3 pid4 1 2 3 4 *SET_PART_LIST $# sid 20 $# pid1 pid2 1 2 *DEFINE_CPM_CHAMBER $# id nchm 1234 2 $# sid1 sid2 ninter chm_id 20 0 1 998 $# sid3 itype3 tochm 2 0 997 $# sid1 sid2 ninter chm_id 1 20 1 997 $# sid3 itype3 tochm 2 0 998 2. Particles with different chamber ID will not interact in particle to particle collision. This feature will allow program to distinguish particles separated by a thin wall. 3. All chambers data are output to lsda binout database. The utility “l2a” can convert it into abstat_chamber ASCII file and process with lsprepost under abstat format *DEFINE_CPM_GAS_PROPERTIES Purpose: To define extended gas thermodynamic properties Card 1 Variable 1 ID 2 3 4 5 6 7 8 Xmm Cp0 Cp1 Cp2 Cp3 Cp4 Type I F F Default none none 0. Card 1 1 Variable μt0 Type F Default 0. 2 μt1 F 0. 3 μt2 F 0. F 0. 4 μt3 F 0. F 0. F 0. F 0. 5 6 7 8 μt4 Chm_ID Vini F 0. I 0 F 0. VARIABLE DESCRIPTION ID Unique ID for this card Xmm Molar mass Cp0, …, Cp4 Coefficients of temperature dependent specific heat with constant pressure Cp(T) = Cp0 + Cp1 T + Cp2 T2 + Cp3 T3 + Cp4 T4 μt0, …, μt4 Coefficients of temperature dependent Joule-Thomson effect μt(T) = μt0 + μt1 T + μt2 T2 + μt2 T3 + μt2 T4 Chm_ID Chamber ID (remark 1) Vini Initial volume for user defined inflator (remark 1) Example: *AIRBAG_PARTICLE $====1====$====2====$====3====$====4====$====5====$====6====$====7====$====8==== 1010 1 1011 1 0 0.0 0.0 1 100000 0 1 300.0 1.0e-04 1 1 1 1 61 0 1.0 0 0 1 0.0 1.0E-04 300.0 -9900 651 653 -9910 3000001 1.0 $==================================================== *DEFINE_CPM_GAS_PROPERTIES $====1====$====2====$====3====$====4====$====5====$====6====$====7====$====8==== 9900 2.897E-02 2.671E+01 7.466E-03-1.323E-06 9910 4.0E-03 20.79 -610.63 -0.0926 Remark: 1.If Chm_ID and Vini are defined. This gas property will be used in the user_ inflator routine which is provided in the dyn21b.f of general usermat package. The code will give current chamber volume, pressure, temperature and time step and expect returning value of change of chamber, burned gas temperature and mass flow rate to feedback to the code for releasing particles. All state data for this chamber will be output binout under abstat_chamber subdirectory. Purpose: To define extended vent hole options *DEFINE_CPM_VENT Card 1 Variable 1 ID 2 3 4 5 6 7 8 C23 LCTC23 LCPC23 ENH_V PPOP C23UP IOPT Type I F I I I F F Default none none none none none none none Card 2 Variable Type Default 1 JT I 0 2 3 4 5 6 7 8 IDS1 IDS2 IOPT1 PID1 IPD2 VANG I I I I I F none none none none none 0. VARIABLE DESCRIPTION ID C23 Unique ID for this card Vent hole coefficient. parameter. (Default 1.0) This is the Wang-Nefske leakage LCTC23 Load curve defining vent hole coefficient as a function of time. LCPC23 ENH_V Load curve defining vent hole coefficient as a function of pressure. Enhance venting option. (Default 0). However if Joule-Thomson effect is considered, the option will set to 1 automatically. EQ.0: disable EQ.1: enable PPOP Pressure difference between interior and ambient pressure to open the vent hole. Once the vent is open then it will stay open. VARIABLE C23UP DESCRIPTION Scale factor of C23 while switching from CPM to uniform pressure calculation. IOPT Directional venting: EQ.1: In shell normal EQ.2: Against shell normal One-way venting: EQ.10: In shell normal EQ.20: Against shell normal Special vent option:: EQ.100: Enable compression seal vent. Vent area is adjusted according to the formula below. See Remark 1. 𝐴vent = max(𝐴current − 𝐴0, 0) EQ.200: Enable push-out vent. Particle remains active while going through this external vent within the range of 2 times of its characteristic length, 𝑙vent. 𝑙vent = √𝐴vent JT Include the Joule-Thomson effect. When the Joule-Thomson effect is enabled ENH_V is automatically set to 1 (enable). EQ.0: disable EQ.1: use part pressure EQ.2: use chamber pressure IDS1 IDS2 IOPT1 PID1, PID2 JT's up stream condition part ID/chamber ID JT's downstream condition part ID/chamber ID Upstream chamber ID for one-way vent hole. This will help the code to determine the probability function. When specified the vent probability function is evaluated from the difference of local part pressures (between PID1 and PID2) instead of the usual calculation involving the chamber pressure. This option is usually used for vents near a long sleeve which causing unrealistic venting using chamber pressure alone. VANG *DEFINE_CPM_VENT DESCRIPTION Cone angle in degrees. Particle goes through this vent will be redirection based on this angle. This option is only valid with internal vent. GT.0: cone angle (maximum 270) EQ.0: disabled (Default) LT.0: direction follows the vent normal Remarks: 1. Compression Seal Vent Model. In order to evaluate bag state variables correctly, the CPM domain needs to be a closed surface for the volume to be well-defined. If the model contains a flap vent which is free to open and close, this option will correctly maintain the bag’s integrity. Example: *AIRBAG_PARTICLE $====1====$====2====$====3====$====4====$====5====$====6====$====7====$====8==== 1010 1 1011 1 0 0.0 0.0 1 100000 0 1 300.0 1.0e-04 1 1 1 1 61 0 -9910 1.0E-04 300.0 2.897E-2 2.671E+1 7.466E-3 -1.323E-6 1000 1001 4.0E-3 20.79 3000001 1.0 $==================================================== *DEFINE_CPM_VENT $====1====$====2====$====3====$====4====$====5====$====6====$====7====$====8==== 9910 1.0 0 0 1 0.0 1 51 2 *DEFINE Purpose: Define a curve [for example, load (ordinate value) versus time (abscissa value)], often loosely referred to as a load curve. The ordinate may represent something other than a load however, as in the case of curves for constitutive models. In the case of constitutive models, *DEFINE_CURVE curves are rediscretized internally with equal intervals along the abscissa for fast evaluation. Rediscretization is not used when evaluating loading conditions such as pressures, concentrated forces, or displacement boundary conditions . The curve rediscretization algorithm was enhanced for the 2005 release of version 970. In certain cases the new load-curve routines changed the final results enough to disrupt benchmarks. For validated models, such as barriers and occupants, requiring numerical consistency, there are keyword options for reverting to the older algorithms. Available options include: <OPTION> 3858 5434a which correspond to the first releases of version 970 and the 2005 release, respectively. Since input errors and wrong results are sometimes related to load curve usage, a “Load curve usage” table is printed in the d3hsp file after all the input is read. This table should be checked to ensure that each curve ID is referenced by the option for which the curve is intended. Card 1 1 2 3 4 5 6 7 8 Variable LCID SIDR SFA SFO OFFA OFFO DATTYP LCINT Type I Default none I 0 F 1. F 1. F 0. F 0. I 0 I Point Cards. Put one pair of points per card (2E20.0). Input is terminated at the next keyword (“*”) card. Card 2… 1 2 3 4 5 6 7 8 Variable A1 O1 Type E20.0 E20.0 Default 0.0 0.0 VARIABLE LCID SIDR SFA SFO OFFA OFFO DESCRIPTION Load curve ID. Tables and load curves may not share common ID's. LS-DYNA allows load curve ID's and table ID's to be used interchangeably. A unique number has to be defined. Flag controlling use of curve during dynamic relaxation. SIDR set to 1 or 2 will activate a dynamic relaxation phase unless IDR- FLG = -999 in *CONTROL_DYNAMIC_RELAXATION. EQ.0: load curve used in normal analysis phase only or for other applications, EQ.1: load curve used in dynamic relaxation phase but not the normal analysis phase, EQ.2: load curve applies to both dynamic relaxation phase and normal analysis phase. Scale factor for abscissa value. This is useful for simple modifications. EQ.0.0: default set to 1.0. Scale factor for ordinate value (function). This is useful for simple modifications. EQ.0.0: default set to 1.0. Offset for abscissa values, see explanation below. Offset for ordinate values (function), see explanation below. DATTYP *DEFINE DESCRIPTION Data type. This affects how offsets are applied . EQ.-2: for fabric stress vs. strain curves (*MAT_FABRIC) as described below. EQ.0: general case for time dependent curves, force versus displacement curves and stress strain curves EQ.1: for general (𝑥, 𝑦) data curves whose abscissa values do not increase monotonically EQ.6: for general (𝑟, 𝑠) data (coordinates in a 2D parametric space) whose values do not increase monotonically. Use for definition of trimming polygons for trimmed NURBS (*ELEMENT_SHELL_NURBS_PATCH, NL.GT.0) LCINT The number of discretization points to use for this curve. If 0 is input, the value of LCINT from *CONTROL_SOLUTION will be used. A1, A2, … Abscissa values. See remarks below. O1, O2, … Ordinate (function) values. See remarks below. Remarks: 1. Warning Concerning Rediscretization. For constitutive models, LS-DYNA internally rediscretizes the curve with uniform spacing to bypass searching during evaluations. The major drawback of this algorithm is that any detail in the curve on a scale finer than the uniform rediscretization grid will be smoothed-out and lost. It is, therefore, important to avoid placing a single point off at some value approaching infinity. The lone point at infinity will cause the resolu- tion of the uniform grid to be coarse relative to the other points, causing the rediscretized curve to be, possibly, featureless. Therefore, when defining curves for constitutive models, points should be spaced as uniformly as possible. Also, since the constitutive model curves are extrapolated, it is important to ensure that extrapolation does not lead to physi- cally meaningless values, such as a negative flow stress. Conversely, extrapola- tion can be exploited to control the results of evaluations at points far from the input data. The number of points in each rediscretized curve is controlled by the parameter LCINT in *CONTROL_SOLUTION. By changing LCINT to a value greater than the default of 100, the rediscretized curves may better resemble the input curves. The data points of the rediscretized curves are written to messag and d3hsp if the parameter IPCURV is set to 1 in *CONTROL_OUTPUT. 2. Scaling. The load curve values are scaled after the offsets are applied, i.e.: Abscissa value = SFA × (Defined value + OFFA) Ordinate value = SFO × (Defined value + OFFO) 3. DATTYP. The DATTYP field controls how the curve is processed during the calculation. a) For DATTYP = 0 positive offsets may be used when the abscissa repre- sents time, since two additional points are generated automatically at time zero and at time 0.999 × OFFA with the function values set to zero. b) If DATTYP = 1, then the offsets do not create these additional points. Negative offsets for the abscissa simply shifts the abscissa values without creating additional points. c) For *MAT_FABRIC material with FORM = 4, 14, -14, or 24, set DATYP = - 2 to define stress vs. strain curves using engineering stress and strain ra- ther the 2nd Piola-Kirchhoff stress and Green strain. 4. Context Dependent Extrapolation. Load curves are not extrapolated by LS- DYNA for applied loads such as pressures, concentrated forces, displacement boundary conditions, etc. Function values are set to zero if the time, etc., goes off scale. Therefore, extreme care must be observed when defining load curves. In the constitutive models, extrapolation is employed if the values on the ab- scissa go off scale. 5. Restart. The curve offsets and scale factors are ignored during restarts if the curve is redefined. See *CHANGE_CURVE_DEFINITION in the restart section. *DEFINE_CURVE_BOX_ADAPTIVITY Purpose: To define a polygon adaptive box in sheet metal forming, applicable to shell elements. This keyword is used together with *CONTROL_ADAPTIVE. Other related keyword is *DEFINE_BOX_ADAPTIVE. Card 1 Variable 1 ID 2 3 4 5 6 7 8 PID LEVEL DIST1 Type I I I F Default none none none none Point Cards. Include as many as necessary. This input ends at the next keyword (“*”) card. Card 2 1 2 3 4 5 6 7 8 Variable Type X F Y F Z F Default none none none VARIABLE DESCRIPTION ID Curve ID; must be unique. The curve must be closed: its first and last point must coincide. PID Sheet blank Part ID, as in *PART. LEVEL Adaptive refinement levels, similar to ‘MAXLVL’ in *CON- TROL_ADAPTIVE. DIST1 *DEFINE_CURVE_BOX_ADAPTIVITY DESCRIPTION Extended depths in Z for a polygon box defined by Card 2, 3, 4, etc. Currently this variable must be input as a negative value. The box depth in Z will be extended in –Z direction by Zmin- abs(DIST1) and in +Z direction by Zmax+abs(DIST1). The XYZ data pairs formed with Card 2, 3, 4, etc. will be automatically closed to create the polygon box. Zmin and Zmax are the minimum and maximum Z-coordinates in all the data pairs. X Y Z X-coordinate of a point on the curve. Y-coordinate of a point on the curve. Z-coordinate of a point on the curve. Remarks: Within the polygon, the variable LEVEL has priority over MAXLVL in *CONTROL_- ADAPTIVE but limited to minimum element size controlled by ADPSIZE. A larger LEVEL (than MAXLVL) value will enable more mesh refinement within the polygon, up to the size defined by ADPSIZE, while meshes outside of the box refined less by a smaller MAXLVL value. However, mesh refinement when LEVEL > MAXLVL is not recommended. The appropriate way of using this keyword (and *DEFINE_BOX_- ADAPTIVE) is to define the polygon box excluding the local areas of interest so refinement inside the local areas will be controlled by MAXLVL while outside of the area to be controlled by LEVEL, and in this case MAXLVL > LEVEL, as shown in Figure 15-9. The advantage of using this keyword is obvious when compared with multiple boxes needed when defining local adaptive refinement with keyword *DEFINE_BOX_- ADPATIVE (Figure 15-10). It is noted that ADPSIZE is a “global” variable, meaning final refined element sized, regardless of the values set for MAXLVL or LEVEL, cannot be smaller than what is defined by ADPSIZE. The 3-D curve (closed polygon) defined by XYZ data pairs should be near the sheet blank in Z after the blank is auto-positioned in the beginning of a simulation. Similar to *DEFINE_BOX_ADAPTIVE, only the elements on the sheet blank initially within the polygon will be considered for use with this keyword. Local coordinate system is not supported at the moment. The 3-D curve can be converted from IGES format to format required here following the procedure outlined in keyword *INTERFACE_BLANKSIZE_{OPTION}. A partial keyword example is provided below, where inside the polygon mesh has no refinement (LEVEL = 1), while outside of the box the mesh is refined 5 levels (MAXLVL = 5). The final minimum element size is defined as 0.4. It is noted that the first point and last point of the polygon are the same, closing the polygon box. *CONTROL_ADAPTIVE $ ADPFREQ ADPTOL ADPOPT MAXLVL TBIRTH TDEATH LCADP IOFLAG &adpfq1 5.0 2 5 0.0 1.000E+20 1 $ ADPSIZE ADPASS IREFLG ADPENE ADPTH MEMORY ORIENT MAXEL 0.4 1 0 &lookfd 0.0 0 0 $ IADPE90 NCFREQ IADPCL ADPCTL CBIRTH CDEATH LCLVL -1 $---+----1----+----2----+----3----+----4----+----5----+----6----+----7----+----8 *DEFINE_CURVE_BOX_ADAPTIVITY $ ID PID LEVEL DIST1 99 1 1 -25.0 $(3E20.0): -59.573399 -6.698870 -40.224651 -90.728516 24.456253 -40.224651 ... -23.213169 18.088070 -10.954337 14.353654 16.130911 -10.954337 -31.070744 -5.785467 -40.487387 -59.573399 -6.698870 -40.224651 Revision information: This feature is available in SMP only, and in LS-DYNA Revision 81918 and later releases. Zmax+abs(DIST1) Adaptivity within the polygon is controlled by LEVEL in *DEFINE_CURVE_BOX_ADAPTIVITY Zmin - abs(DIST1) Adaptivity in flanging area outside of the polygon is controlled by MAXLVL in *CONTROL_ADAPTIVE, and MAXLVL > LEVEL. Figure 15-9. Defining an adaptive polygon box Adaptivity within these boxes is controlled by LEVEL in *DEFIN_BOX_ADAPTIVE Adaptivity in flanging area along the hood line is controlled by MAXLVL in *CONTROL_ADAPTIVE, and MAXLVL > LEVEL. Figure 15-10. Defining adaptive boxes *DEFINE_CURVE_COMPENSATION_CONSTRAINT_OPTION Purpose: This keyword with the two options allows for the definition of a localized die face region for springback compensation of stamping tools. Options available include: BEGIN END NOTE: *DEFINE_CURVE_COMPENSATION_CONSTRAINT_BEGIN and *DEFINE_CURVE_COMPENSATION_CONSTRAINT_END are not valid in the context of a general keyword input deck. In- stead, they may only be used inside of an *INCLUDE_COMPEN- SATION_CURVE include file. The required option, which must be either BEGIN or END, distinguishes between two different closed curves, which, when taken together identify a portion of the die wherein springback compensation is applied, and a transition region for which compensation smoothly tapers off. Card 1 1 2 3 4 5 6 7 8 Variable CRVID INOUT TYPE Type Default I 0 I 0 I none Point Cards. Include as many as necessary (3E16.0). This input ends at the next keyword (“*”) card. Only the projection of this curve onto the 𝑥-𝑦 plane is used. Card 2 1 2 3 4 5 6 7 8 Variable Type X F Y F Z F Default 0.0 0.0 0.0 A perfect sphere surface An area of impection (to be compensated) Section A-A Begin curve Transition area End curve VARIABLE CRVID Figure 15-11. Local area compensation. DESCRIPTION Curve ID; must be unique. The curve must be closed: its first and last point must coincide. INOUT Flag to indicate local area to be compensated: EQ.0: For this option, the compensated region of the die consists of all points for which the projection onto the 𝑥-𝑦 plane is exterior to the projection of the BEGIN curve. The projection of the END curve is assumed exterior to the BEGIN curve. The transition region, then, consists of all die points for which the projection is between the BEGIN and END curves. All other points on the die are uncompensated. EQ.1: For this option, the compensated region of the die consists of all points for which the projection onto the 𝑥-𝑦 plane is interior to the projection of the BEGIN curve. The projection of the END curve is assumed exterior to the BEGIN curve. The transition region, then, consists of all die points for which the projection is between the BEGIN and END curves. All other points on the die are uncompensated. See Figure 15-11. TYPE Type code - must be “0”. X Y 𝑥-coordinate of a point on the curve. 𝑦-coordinate of a point on the curve. *DEFINE_CURVE_COMPENSATION_CONSTRAINT DESCRIPTION Z 𝑧-coordinate of a point on the curve. Motivation: Sometimes springback occurs in a localized region of the die face. Since other parts of the die face are better left undisturbed, a localized compensation makes the most sense to bring the part shape back to the design intent. A typical such example will be the front portion along the grill and headlamp, or the rear portion along the windshield of a trimmed hood inner panel. A decklid (or trunk lid) inner also exhibits the similar needs. Once the localized areas are identified, iterative compensation scheme may be employed within this localized region to bring the springback panel back to design shape. Modeling details: Referring to Figure 15-11, the keywords *COMPENSATION_CONSTRAINT_BEGIN and *COMPENSATION_CONSTRAINT_END must be used together in a file, which in turn will be included in keyword *INCLUDE_COMPENSATION_CURVE. The keyword “BEGIN” precedes the keyword “END”, each is defined by discrete points. In addition, each curve must form a closed loop. The area formed between the two curves is a transition area, and will be affected in the compensated tooling. LS-PrePost4.0 under Curve → Merge → Multiple Method, multiple disconnected curves can be joined together, and output in “.xyz” format required here. The curve can be a 3-D piecewise linear curve with coordinates in 𝑥, 𝑦 and 𝑧. However, 𝑧-coordinates are ignored; meaning the tooling to be compensated must be positioned so draw direction is in global 𝑧; otherwise error will occur. In addition, it is assumed that both “blank before springback” and “blank after springback” will be smaller than rigid tools in dimension. It is further noted the rigid tool meshes should be discretized fine enough to provide enough degrees of freedom for the compensation. Application example – single region: A complete input deck is provided below for a local compensation simulation. The keyword files state1.k and state2.k consist model (nodes and elements) information of the blank before and after springback, respectively. It is noted here that if the blank is adaptively refined, the adaptive constraints must be included in the keyword files. The keyword file tools.k consists the stamping tools (with PID 1, 2, 3 and 4) all positioned in home position. The keyword file curvesxy.xyz consists keywords “BEGIN” and “END” defining the two closed-loop curves used to define a localized area. *KEYWORD *TITLE LS-Dyna971 Compensation Job $---+----1----+----2----+----3----+----4----+----5----+----6----+----7----+----8 *INTERFACE_COMPENSATION_NEW $ METHOD SL SF ELREF PSIDm UNDCT ANGLE NOLINEAR 6 10.000 0.700 0 1 0 0 1 *INCLUDE_COMPENSATION_BLANK_BEFORE_SPRINGBACK state1.k *INCLUDE_COMPENSATION_BLANK_AFTER_SPRINGBACK state2.k *INCLUDE_COMPENSATION_DESIRED_BLANK_SHAPE state1.k *INCLUDE_COMPENSATION_COMPENSATED_SHAPE state1.k *INCLUDE_COMPENSATION_CURRENT_TOOLS tools.k *INCLUDE_COMPENSATION_CURVE curvesxy.xyz *SET_PART_LIST 1 1,2,3,4 *END A portion of the file curvesxy.xyz is shown below, *KEYWORD *DEFINE_CURVE_COMPENSATION_CONSTRAINT_BEGIN $ CID IN/OUT TYPE 1 1 0 -1.86925e+02 1.83338e+03 -1.55520e+01 -1.83545e+02 1.83003e+03 -1.55469e+01 -1.80162e+02 1.82668e+03 -1.55428e+01 -1.91811e+02 1.83884e+03 -1.56014e+01 -1.90187e+02 1.83701e+03 -1.55852e+01 -1.88560e+02 1.83519e+03 -1.55688e+01 -1.86925e+02 1.83338e+03 -1.55520e+01 *DEFINE_CURVE_COMPENSATION_CONSTRAINT_END $ CID IN/OUT TYPE 2 1 0 -4.07730e+02 1.61371e+03 -8.04858e+01 -3.84480e+02 1.59890e+03 -7.99169e+01 -3.61193e+02 1.58423e+03 -7.93471e+01 -3.37832e+02 1.56984e+03 -7.87756e+01 -4.49289e+02 1.67556e+03 -8.04582e+01 -4.35672e+02 1.65473e+03 -8.05162e+01 -4.21764e+02 1.63396e+03 -8.05530e+01 -4.07730e+02 1.61371e+03 -8.04858e+01 *END Compensated tool Target mesh Springback mesh Section A-A Figure 15-12. Local compensation details. It is noted the first point and last point are exactly the same, forming a closed loop. In Figure 15-11, local area compensation is to be performed in the center portion of a rigid sphere. Based on springback and target meshes, the compensated tool mesh is obtained and smooth transition areas are achieved, Figure 15-12. Here the compensation scale factor of 0.7 is used. Application example – multiple regions: Multi-region localized compensation is also possible by defining multiple pairs of the BEGIN and END versions of this keyword, each forming a localized region. For example, for localized compensation of two regions, the file curvesxy.xyz will read as follows, *KEYWORD *DEFINE_CURVE_COMPENSATION_CONSTRAINT_BEGIN $ CID IN/OUT TYPE 1 1 0 3.67967e+02 1.63423e+03 -6.98532e+01 3.60669e+02 1.62992e+03 -6.92921e+01 3.53586e+02 1.62525e+03 -6.88777e+01 ⋮ ⋮ ⋮ *DEFINE_CURVE_COMPENSATION_CONSTRAINT_END $ CID IN/OUT TYPE 2 1 0 4.12534e+02 1.75537e+03 -5.83975e+01 3.98853e+02 1.75264e+03 -5.58860e+01 3.85292e+02 1.74921e+03 -5.35915e+01 ⋮ ⋮ ⋮ *DEFINE_CURVE_COMPENSATION_CONSTRAINT_BEGIN $ CID IN/OUT TYPE 3 1 0 -4.37478e+02 2.67393e+03 -1.70421e+02 -4.45605e+02 2.67209e+03 -1.71724e+02 -4.53649e+02 2.66985e+03 -1.72894e+02 ⋮ ⋮ ⋮ *DEFINE_CURVE_COMPENSATION_CONSTRAINT_END $ CID IN/OUT TYPE 4 1 0 -4.49426e+02 2.79057e+03 -2.18740e+02 -4.63394e+02 2.78749e+03 -2.20955e+02 Section B-B Compensated tool Target mesh Section B-B Springback mesh Figure 15-13. Multi-region local compensation. -4.77223e+02 2.78370e+03 -2.22938e+02 ⋮ *END ⋮ ⋮ Figure 15-13 (top) shows an example of two localized areas of the sphere to be compensated. The compensation results are shown in Figure 15-13 (bottom). Again, a compensation scale factor of 0.7 was used and smooth transition areas are achieved. Revision information: This feature is available in double precision version of LS-DYNA starting in Revision 62038. Multi-region localized compensation is available starting in Revision 66129 and later releases. In addition, prior to Revision 66129, all keywords must be capitalized. Also, official release version starting in R7.1.1 (double precision) can be used. *DEFINE_CURVE_DRAWBEAD Purpose: This keyword simplifies the definition of a draw bead, which previously required the use of many keywords. NOTE: This option has been deprecated in favor of *DE- FINE_MULTI_DRAWBEADS_IGES. Card 1 1 2 3 4 5 6 7 8 Variable CID TCTYPE VID PID BLKID PERCT LCID Type I I I I I F I Default none none none none none 0.0 none Point Cards. For TCTYPE = 1 define points on the curve. Input is terminated at the next keyword (“*”) card. 4 5 6 7 8 Card 2 Variable 1 CX Type F 2 CY F 3 CZ Default 0.0 0.0 IGES Card. For TCTYPE = 2 set an IGES file. Card 2 1 2 3 4 5 6 7 8 Variable Type Default FILENAME C none VARIABLE DESCRIPTION CID Draw bead curve ID; must be unique. TCTYPE Flag to indicate input curve data format: EQ.1: XYZ data, EQ.2: IGES format data. VID PID Vector ID, as defined by *DEFINE_VECTOR. This vector is used to project the supplied curves to the rigid tool, defined by the PID below. Part ID of a rigid tool to which the curves are projected and attached. BLKID Part ID of the blank. PERCT Draw bead lock percentage or draw bead force. GT.0: Percentage of the full lock force for the bead defined. This is the ratio of desired restraining force over the full lock force. The value should be between 0.0 and 100.0. LT.0: Absolute value is the draw bead force. LCID Load curve ID defining material hardening curve of the sheet blank, BLKID. CX, CY, CZ Points on the curve. FILENAME IGES file name. Remarks: 1. This feature implements the following input algorithm for drawbeads: a) It reads a draw bead curve in either XYZ or IGES format b) projects the curve to the rigid tool specified c) creates extra node set and attaches it to the rigid tool. d) With supplied material hardening curve (LCID), full lock force is calculat- ed. There is no need to define *CONTACT_DRAWBEAD and *CONSTRAINED_- RIGID_BODIES since they are treated internally within the code. 2. The “curve” menu in LS-PrePost can be used to break or join multiple disconnected curves, and output in either ‘XYZ’ or IGES format. 3. The following partial keyword example defines a draw bead curve ID 98 (IGES file “bead1.iges”) to restrain blank part ID 63. Full lock force is calculated from the strain hardening curve ID 400. The draw bead is projected along vector ID 991, and is attached to a rigid tool of part ID 3. $---+----1----+----2----+----3----+----4----+----5----+----6----+----7----+--- -8 *KEYWORD *DEFINE_VECTOR 991,0.0,0.0,0.0,0.0,0.0,10.0 *DEFINE_CURVE_DRAWBEAD $ CID TCTYPE VID PID BLKID PERCT LCID 98 2 991 3 63 52.442 400 bead1.iges *MAT_037 $ MID R0 E PR SIGY ETAN R HCLID 1 7.89E-09 2.00E+05 0.3 240.0 1.6 400 *DEFINE_CURVE 400 0.0,240.0 0.02,250.0 ... 1.0, 350.0 *END Revision information: This feature is available starting in LS-DYNA R5 Revision 62464. *DEFINE Purpose: Define a curve by optionally scaling and offsetting the abscissa and ordinates of another curve defined by the *DEFINE_CURVE keyword. Card 1 1 2 3 4 5 6 7 8 Variable LCID RLCID SFA SFO OFFA OFFO Type I I F Default none none 1. F 1. F 0. F 0. VARIABLE LCID DESCRIPTION Load curve ID. Tables and load curve ID’s must be unique. RLCID Reference load curve ID. SFA SFO OFFA OFFO Scale factor for abscissa value of curve ID, RLCID. This value scales the SFA value defined for RLCID. EQ.0.0: default set to 1.0. Scale factor for ordinate value (function) of curve ID, RLCID. This value scales the SFO value defined for RLCID. EQ.0.0: default set to 1.0. Offset for abscissa values. This value is added to the OFFA value defined for RLCID. Offset for ordinate values (function). This value is added to the OFFO value defined for RLCID. *DEFINE_CURVE_ENTITY Purpose: Define a curve of straight line segments and circular arcs that defines an axisymmetric surface. This curve can only be used with the keyword, *CONTACT_EN- TITY for the load curve entity, GEOTYP = 11. Card 1 2 3 4 5 6 7 8 Variable LCID SFA SFO SFR OFFA OFFO OFFR Type I F Default none 1. F 1. F 1. F 0. F 0. F 0. Point Cards. Put one point per card (3E20.0,I20). Include as many cards as needed Input is terminated when a “*” card is found. Card 1 2 3 4 5 6 7 8 Variable Type Ai F Oi F Ri F Default 0.0 0.0 optional IFLAG I Required if |R1| > 0 VARIABLE LCID DESCRIPTION Load curve ID. Tables and load curves may not share common ID's. LS-DYNA allows load curve ID's and table ID's to be used interchangeably. A unique number has to be defined. SFA Scale factor for axis value. This is useful for simple modifications. EQ.0.0: default set to 1.0. SFO Scale factor for radius values. modifications. This is useful for simple EQ.0.0: default set to 1.0. VARIABLE SFR DESCRIPTION Scale factor for circular radius. This is useful for simple modifications. EQ.0.0: default set to 1.0. Offset for axis values, see explanation below. Offset for radius values, see explanation below. Offset for circular radius, see explanation below. Z-axis coordinates along the axis of rotation. Radial coordinates from the axis of rotation Radius of arc between points (Ai,Oi) and (Ai+1,Oi+1). If zero, a straight line segment is assumed. Defined if |Ri| > 0. Set to 1 if center of arc is inside axisymmetric surface and to -1 if the center is outside the axisymmetric surface. OFFA OFFO OFFR Ai Oi Ri IFLAG Remarks: 1. The load curve values are scaled after the offsets are applied, i.e.: Axis value = SFA × (Defined value + OFFA) Radius value = SFO × (Defined value + OFFO) Circular value = SFR × (Defined value + OFFR) *DEFINE_CURVE_FEEDBACK Purpose: Define information that is used as the solution evolves to scale the ordinate values of the specified load curve ID. This keyword is usually used in connection with sheet metal forming calculations. Card 1 1 2 3 4 5 6 7 8 Variable LCID PID BOXID FLDID Type I I Default none none Card 2 1 2 I 0 3 I none 4 5 6 7 8 Variable FSL TSL SFF SFT BIAS Type F F F F F Default none none 1.0 1.0 0.0 VARIABLE DESCRIPTION LCID PID BOXID FLDID FSL TSL ID number for load curve to be scaled. Active part ID for load curve control Box ID. Elements of specified part ID contained in box are checked. If the box ID is set to zero the all elements of the active part are checked. Load curve ID which defines the flow limit diagram as shown in Figure 15-14. If the ratio, 𝑟 = εmajorworkpiece factor for flow, SFF, is active. ⁄ 𝜀majorfld exceeds FSL, then scale Thickness strain limit. If the thickness strain limit is exceeded, then the scale factor for thickening, SFT, is active. εmnr = 0 PLANE STRAIN εmjr 80 70 60 50 40 30 20 10 % εmnr εmjr εmnr εmjr DRAW STRETCH -50 -40 -30 -20 -10 +10 +20 +30 +40 +50 % MINOR STRAIN Figure 15-14. Flow limit diagram. VARIABLE DESCRIPTION Scale factor for the flow limit diagram. Scale factor for thickening. Bias for combined flow and thickening. Bias must be between -1 and 1. SFF SFT BIAS Remarks: This feature scales the ordinate values of a load curve according to a computed scale factor, 𝑆𝑓 , that depends on both the major strain, r, and the through thickness, t. At each time step the load curve is scaled by 𝑆𝑓 according to, 𝑛+1 𝑆scaled load curve = Sf(𝑟, 𝑡) × 𝑆load curve , where the superscript denotes the time step. The scale factor depends on r, which is a strain measure defined as, 𝑟 = εmajorworkpiece 𝜀majorfld . The scale factor, then, is given by, 𝑆𝑓 = ⎧1 {{{ ⎨ {{{ ⎩ SFF SFT (1 − BIAS)×SFF + 𝑟 < FSL, 𝑡 < TSL 𝑟 > FSL, 𝑡 < TSL 𝑟 < FSL, 𝑡 > TSL (1 + BIAS) × SFT 𝑟 > FSL, 𝑡 > TSL Usually SFF is slightly less than unity and SFT is slightly greater than unity so that 𝑆load curve changes insignificantly from time step to time step. *DEFINE Purpose: This keyword allows for defining Forming Limit Diagram (FLD) using sheet metal thickness ‘t’ and strain hardening value ‘n’, applicable to shell elements only. This feature is available in LS-DYNA Revision 61435 and later releases. 4 5 6 7 8 Card 1 1 Variable LCID Type I 2 TH F 3 TN F Default none 0.0 0.0 VARIABLE DESCRIPTION LCID Load curve ID. Sheet metal thickness. Strain hardening value of the sheet metal, as in power law (Swift). TH TN Remarks: 1. This keyword is used in conjunction with keyword *MAT_TRANSVERSELY_- ANISOTROPIC_ELASTIC_PLASTIC_NLP_FAILURE, and for shell elements only. For detailed formula of calculating the FLD based on sheet metal thick- ness and n-value, please refer to the following paper: Ming F. Shi, Shawn Ge- lisse, “Issues on the AHSS Forming Limit Determination”, IDDRG 2006. 2. 3. It is noted that this FLD calculation method is limited to sheet metal steels with thickness equal to or less than 2.5 mm, and it is not suitable for aluminum sheets. In a validation example shown in Figure 15-15, a single shell element is stretched in three typical strain paths (linear): uniaxial, plane strain and equi- biaxial. Strain limits for each path are recovered when the history variable (Formability Index limit in *MAT_037) reaches 1.0, shown in Figure 15-16. The top most point (strain limit) of each strain path coincides with the FLC curve calculated according to the paper, indicating the FLC defined by this keyword is working correctly. As shown in a partial keyword file below, the FLC is defined using a thickness value of 1.5 and n-value of 0.159. The ‘LCID’ of 891 is used to define a variable ‘ICFLD’ in keyword *MAT_TRANSVERSELY_- ANISOTROPIC_ELASTIC_PLASTIC_NLP_FAILURE. *MAT_TRANSVERSELY_ANISOTROPIC_ELASTIC_PLASTIC_NLP_FAILURE $ MID RO E PR SIGY ETAN R HLCID 1 7.830E-09 2.070E+05 0.28 0.0 0.0 -0.864 200 $ IDY EA COE ICFLD 891 *DEFINE_CURVE_FLC $ LCID, TH, TN 891,1.5,0.159 $ DP600 NUMISHEET'05 Xmbr, Power law fitted *DEFINE_CURVE 200 0.000,395.000 0.001,425.200 0.003,440.300 ... 4. For aluminum sheets, *DEFINE_CURVE can be used to input the FLC for the variable ‘ICFLD’ in *MAT_TRANSVERSELY_ANISOTROPIC_ELASTIC_PLAS- TIC_NLP_FAILURE. x i a l n i a Plane strain Equibiaxial Shell Unstrained Figure 15-15. A single shell strained in three different strain paths Single Element Test Uniaxial Equi-biaxial Plane Strain Calculated FLC 1 0.8 0.6 0.4 0.2 0 -0.6 -0.4 -0.2 0 0.2 0.4 Minor True Strain Figure 15-16. Validation of the FLC defined by this keyword *DEFINE_CURVE_FUNCTION Purpose: Define a curve [for example, load (ordinate value) versus time (abscissa value)] where the ordinate is given by a function expression. The function can reference other curve definition, kinematical quantities, forces, interpolating polynomials, intrinsic functions, and combinations thereof. Please note that many functions require the definition of a local coordinate system . To output the curve to an ASCII database, see *DATABASE_CURVOUT. This command is not for defining curves for material models. Note that arguments appearing in square brackets “[ ]” are optional. Card 1 2 3 4 5 6 7 8 Variable LCID SIDR Type I Default none I 0 Function Cards. Insert as many cards as needed. These cards are combined to form a single line of input. The next keyword (“*”) card terminates this input. Card 1 2 3 4 5 6 7 8 Variable Type Remarks VARIABLE LCID FUNCTION A80 1 DESCRIPTION Load curve ID. Tables and load curves may not share common ID's. LS-DYNA allows load curve ID's and table ID's to be used interchangeably. A unique number has to be defined. VARIABLE DESCRIPTION SIDR Stress initialization by dynamic relaxation: EQ.0: load curve used in transient analysis only or for other applications, EQ.1: load curve used in stress initialization but not transient analysis, EQ.2: load curve applies to both initialization and transient analysis. FUNCTION Arithmetic expression involving a combination of the following possibilities. Constants and Variables: FUNCTION DESCRIPTION TIME Current simulation time TIMESTEP Current simulation time step PI DTOR RTOD Proportionality constant relating the circumference of a circle to its diameter Degrees to radians conversion factor (𝜋/180) Radians to degrees conversion factor (180/𝜋) Intrinsic Functions: FUNCTION DESCRIPTION ABS(𝑎) Absolute value of 𝑎 AINT(𝑎) Nearest integer whose magnitude is not larger than a ANINT(𝑎) Nearest whole number to a MOD(𝑎1, 𝑎2) Remainder when 𝑎1 is divided by 𝑎2 SIGN(𝑎1, 𝑎2) Transfer sign of 𝑎2 to magnitude of 𝑎1 MAX(𝑎1, 𝑎2) Maximum of 𝑎1 and 𝑎2 MIN(𝑎1, 𝑎2) Minimum of 𝑎1 and 𝑎2 *DEFINE_CURVE_FUNCTION DESCRIPTION SQRT(𝑎) Square root of 𝑎 EXP(𝑎) LOG(𝑎) 𝑒 raised to the power of 𝑎 Natural logarithm of 𝑎 LOG10(𝑎) Log base 10 of 𝑎 SIN(𝑎) COS(𝑎) Sine of 𝑎 Cosine of 𝑎 TAN(𝑎) Tangent of 𝑎 ASIN(𝑎) Arc sine of 𝑎 ACOS(𝑎) Arc cosine of 𝑎 ATAN(𝑎) Arc tangent of 𝑎 ATAN2(𝑎1, 𝑎2) Arc tangent of 𝑎1/𝑎2 SINH(𝑎) Hyperbolic sine of 𝑎 COSH(𝑎) Hyperbolic cosine of 𝑎 TANH(𝑎 ) Hyperbolic tangent of 𝑎 Load Curves: FUNCTION LCn DESCRIPTION Ordinate value of curve n defined elsewhere FUNCTION DESCRIPTION DELAY(LC𝑛, 𝑡delay, 𝑦def) Delays curve 𝑛, defined by *DEFINE_CURVE_FUNC- TION, *DEFINE_FUNCTION or DEFINE_CURVE, by Tdelay when simulation time ≥ Tdelay, and sets the delayed curve value to Ydef when time < Tdelay, i.e., 𝑓delay(𝑡) = {⎧ 𝑓 (t− 𝑡delay) ⎩{⎨ 𝑦def 𝑡 ≥ 𝑡delay 𝑡 < 𝑡delay For a nonlinear curve, a Tdelay equal to more than 5,000 time steps might compromise the accuracy and must be used with caution. When Tdelay is a negative integer, delay time is input in terms of time step. |Tdelay| is the number of delay time steps. In such case, |Tdelay| is limited to a maximum of 100. For example, Tdelay = -2 delays the curve by 2 time steps. Coordinate Functions: FUNCTION DESCRIPTION CX(𝑛) CY(𝑛) CZ(𝑛) Value of 𝑥-coordinate for node 𝑛. Value of 𝑦-coordinate for node 𝑛. Value of 𝑧-coordinate for node 𝑛. Displacement Functions: FUNCTION DM(𝑛1[, 𝑛2]) DESCRIPTION Magnitude of translational displacement of node 𝑛1 relative to node 𝑛2. Node 𝑛2 is optional and if omitted the displacement is computed relative to ground. DMRB(𝑛) Magnitude of translational displacement of rigid body having a part ID of 𝑛 DX(𝑛1[, 𝑛2, 𝑛3]) DY(𝑛1[, 𝑛2, 𝑛3]) DZ(𝑛1[, 𝑛2, 𝑛3]) DXRB(𝑛) DYRB(𝑛) DZRB(𝑛) AX(𝑛1[, 𝑛2]) AY(𝑛1[, 𝑛2]) AZ(𝑛1[, 𝑛2]) *DEFINE_CURVE_FUNCTION DESCRIPTION 𝑥-translational displacement of node 𝑛1 relative to node 𝑛2 expressed in the local coordinate system of node 𝑛3. In other words, at any time t, the function returns the component of relative displacement that lies in the x-direction of the local coordinate system at time = t. If node 𝑛2 is omitted it defaults to ground. If node 𝑛3 is not specified the displacement is reported in the global coordinate system. 𝑦-translational displacement of node 𝑛1 relative to node 𝑛2 expressed in the local coordinate system of node 𝑛3. In other words, at any time t, the function returns the component of relative displacement that lies in the y-direction of the local coordinate system at time = t. If node 𝑛2 is omitted it defaults to ground. If node 𝑛3 is not specified the displacement is reported in the global coordinate system. 𝑧-translational displacement of node 𝑛1 relative to node 𝑛2 expressed in the local coordinate system of node 𝑛3. In other words, at any time t, the function returns the component of relative displacement that lies in the z-direction of the local coordinate system at time = t. If node 𝑛2 is omitted it defaults to ground. If node 𝑛3 is not specified the displacement is reported in the global coordinate system. 𝑥-translational displacement of rigid body having a part ID of 𝑛 𝑦-translational displacement of rigid body having a part ID of 𝑛 𝑧-translational displacement of rigid body having a part ID of 𝑛 Rotation displacement of node 𝑛1 about the local 𝑥-axis of node 𝑛2. If 𝑛2 is not specified then it defaults to ground. In computing this value it is assumed the rotation about the other two axes (𝑦-, 𝑧-axes) of node 𝑛2 is zero. Rotation displacement of node 𝑛1 about the local 𝑦-axis of node 𝑛2 . If 𝑛2 is not specified then it defaults to ground. In computing this value it is assumed the rotation about the other two axes (𝑥-, 𝑧-axes) of node 𝑛2 is zero. See Remark 1. Rotation displacement of node 𝑛1 about the local 𝑧-axis of node 𝑛2. If 𝑛2 is not specified then it defaults to ground. In computing this value it is assumed the rotation about the other two axes (𝑥-, 𝑦-axes) of node 𝑛2 is zero. See Remark 1. FUNCTION PSI(𝑛1[, 𝑛2]) DESCRIPTION First angle in the body2:313 Euler rotation sequence which orients node 𝑛1 in the frame of node 𝑛2. If 𝑛2 is omitted it defaults to ground. See Remark 1. THETA(𝑛1[, 𝑛2]) Second angle in the body2:313 Euler rotation sequence which orients node 𝑛1 in the frame of node 𝑛2. If 𝑛2 is omitted it defaults to ground. See Remark 1. PHI(𝑛1[, 𝑛2]) Third angle in the body2:313 Euler rotation sequence which orients node 𝑛1 in the frame of node 𝑛2. If 𝑛2 is omitted it defaults to ground. See Remark 1. YAW(𝑛1[, 𝑛2]) First angle in the body3:321 yaw-pitch-roll rotation sequence which orients node 𝑛1 in the frame of node 𝑛2. If 𝑛2 is omitted it defaults to ground. See Remark 1. PITCH(𝑛1[, 𝑛2]) Second angle in the body3:321 yaw-pitch-roll rotation sequence which orients node 𝑛1 in the frame of node 𝑛2. If 𝑛2 is omitted it defaults to ground. See Remark 1. ROLL(𝑛1[, 𝑛2]) Third angle in the body3:321 yaw-pitch-roll rotation sequence which orients node 𝑛1 in the frame of node 𝑛2. If 𝑛2 is omitted it defaults to ground. See Remark 1. Velocity Functions: FUNCTION VM(𝑛1[, 𝑛2]) DESCRIPTION Magnitude of translational velocity of node 𝑛1 relative to node 𝑛2. Node 𝑛2 is optional and if omitted the velocity is computed relative to ground. VR(𝑛1[, 𝑛2]) Relative radial translational velocity of node 𝑛1 relative to node. If node 𝑛2 is omitted it defaults to ground. VX(𝑛1[, 𝑛2, 𝑛3]) 𝑥-component of the difference between the translational velocity vectors of node 𝑛1 and node 𝑛2 in the local coordinate system of node 𝑛3. If node 𝑛2 is omitted it defaults to ground. Node 𝑛3 is optional and if not specified the global coordinate system is used. VY(𝑛1[, 𝑛2, 𝑛3]) VZ(𝑛1[, 𝑛2, 𝑛3]) *DEFINE_CURVE_FUNCTION DESCRIPTION 𝑦-component of the difference between the translational velocity vectors of node 𝑛1 and node 𝑛2 in the local coordinate system of node 𝑛3. If node 𝑛2 is omitted it defaults to ground. Node 𝑛3 is optional and if not specified the global coordinate system is used. 𝑧-component of the difference between the translational velocity vectors of node 𝑛1 and node 𝑛2 in the local coordinate system of node 𝑛3. If node 𝑛2 is omitted it defaults to ground. Node 𝑛3 is optional and if not specified the global coordinate system is used. WM(𝑛1[, 𝑛2]) Magnitude of angular velocity of node 𝑛1 relative to node 𝑛2. Node 𝑛2 is optional and if omitted the angular velocity is computed relative to ground. WX(𝑛1[, 𝑛2, 𝑛3]) WY(𝑛1[, 𝑛2, 𝑛3]) WZ(𝑛1[, 𝑛2, 𝑛3]) 𝑥-component of the difference between the angular velocity vectors of node 𝑛1 and node 𝑛2 in the local coordinate system of node 𝑛3. If node 𝑛2 is omitted it defaults to ground. Node 𝑛3is optional and if not specified the global coordinate system is used. See Remark 1. 𝑦-component of the difference between the angular velocity vectors of node 𝑛1 and node 𝑛2in the local coordinate system of node 𝑛3. If node 𝑛2 is omitted it defaults to ground. Node 𝑛3is optional and if not specified the global coordinate system is used. See Remark 1. 𝑧-component of the difference between the angular velocity vectors of node 𝑛1 and node 𝑛2 in the local coordinate system of node 𝑛3. If node 𝑛2is omitted it defaults to ground. Node 𝑛3is optional and if not specified the global coordinate system is used. See Remark 1. Acceleration Functions: FUNCTION ACCM(𝑛1[, 𝑛2]) DESCRIPTION Magnitude of translational acceleration of node 𝑛1 relative to node 𝑛2. Node 𝑛2 is optional and if omitted the acceleration is computed relative to ground. See Remark 1. FUNCTION ACCX(𝑛1[, 𝑛2, 𝑛3]) ACCY(𝑛1[, 𝑛2, 𝑛3]) ACCZ(𝑛1[, 𝑛2, 𝑛3]) DESCRIPTION 𝑥-component of the difference between the translational acceleration vectors of node 𝑛1 and node 𝑛2 in the local coordinate system of node 𝑛3. If node 𝑛2 is omitted it defaults to ground. Node 𝑛3 is optional and if not specified the global coordinate system is used. See Remark 1. 𝑦-component of the difference between the translational acceleration vectors of node 𝑛1 and node 𝑛2 in the local coordinate system of node 𝑛3. If node 𝑛2 is omitted it defaults to ground. Node 𝑛3is optional and if not specified the global coordinate system is used. See Remark 1. 𝑧-component of the difference between the translational acceleration vectors of node 𝑛1 and node 𝑛2 in the local coordinate system of node 𝑛3. If node 𝑛2 is omitted it defaults to ground. Node 𝑛3 is optional and if not specified the global coordinate system is used. See Remark 1. WDTM(𝑛1[, 𝑛2]) Magnitude of angular acceleration of node 𝑛1 relative to node 𝑛2. Node 𝑛2 is optional and if omitted the angular acceleration is computed relative to ground. See Remark 1. WDTX(𝑛1[, 𝑛2, 𝑛3]) WDTY(𝑛1[, 𝑛2, 𝑛3]) WDTZ(𝑛1[, 𝑛2, 𝑛3]) the difference between the angular 𝑥-component of acceleration vectors of node 𝑛1 and node 𝑛2 in the local coordinate system of node 𝑛3. If node 𝑛2 is omitted it defaults to ground. Node 𝑛3 is optional and if not specified the global coordinate system is used. See Remark 1. the difference between 𝑦-component of the angular acceleration vectors of node 𝑛1and node 𝑛2 in the local coordinate system of node 𝑛3. If node 𝑛2 is omitted it defaults to ground. Node 𝑛3 is optional and if not specified the global coordinate system is used. See Remark 1. the difference between 𝑧-component of the angular acceleration vectors of node 𝑛1 and node 𝑛2 in the local coordinate system of node 𝑛3. If node 𝑛2 is omitted it defaults to ground. Node 𝑛3 is optional and if not specified the global coordinate system is used. See Remark 1. *DEFINE_CURVE_FUNCTION FUNCTION FM(𝑛1[, 𝑛2]) FX(𝑛1[, 𝑛2, 𝑛3]) FY(𝑛1[, 𝑛2, 𝑛3]) FZ(𝑛1[, 𝑛2, 𝑛3]) DESCRIPTION Magnitude of the SPC force acting on node 𝑛1 minus the force acting on node 𝑛2. Node 𝑛2 is optional and if omitted the force that acting only on 𝑛1 Is returned. See Remark 1. 𝑥-component of SPC force acting on node 𝑛1 as computed in the optional local system of node 𝑛3. If 𝑛2 is specified, the force acting on 𝑛2 is subtracted from the force acting on 𝑛1. See Remark 1. 𝑦-component of SPC force acting on node 𝑛1 as computed in the optional local system of node 𝑛3. If 𝑛2 is specified, the force acting on 𝑛2 is subtracted from the force acting on 𝑛1. See Remark 1. 𝑧-component of SPC force acting on node 𝑛1 as computed in the optional local system of node 𝑛3. If 𝑛2 is specified, the force acting on 𝑛2 is subtracted from the force acting on 𝑛1. See Remark 1. TM(𝑛1[, 𝑛2]) Magnitude of SPC torque acting on node 𝑛1 minus the torque acting node 𝑛2. Node 𝑛2 is optional and if omitted the torque that acting only on 𝑛1. See Remark 1. TX(𝑛1[, 𝑛2, 𝑛3]) TY(𝑛1[, 𝑛2, 𝑛3]) TZ(𝑛1[, 𝑛2, 𝑛3]) 𝑥-component of the SPC torque acting on node 𝑛1 as computed in the optional local system of node 𝑛3. If 𝑛2 is specified, the torque acting on 𝑛2 is subtracted from the torque acting on 𝑛1. See Remark 1. 𝑦-component of the SPC torque acting on node 𝑛1 as computed in the optional local system of node 𝑛3. If 𝑛2 is specified, the torque acting on 𝑛2 is subtracted from the torque acting on 𝑛1. See Remark 1. 𝑧-component of the SPC torque acting on node 𝑛1 as computed in the optional local system of node 𝑛3. If 𝑛2 is specified, the torque acting on 𝑛2 is subtracted from the torque acting on 𝑛1. See Remark 1. Sensor Functions: FUNCTION SENSOR(𝑛) DESCRIPTION Returns a value of 1.0 if *SENSOR_CONTROL of control ID 𝑛 has a status of “on”. If the sensor has a status of “off”, then the returned value is equal to the value of the TYPEID field on to *SENSOR_CONTROL when “function,” otherwise SENSOR(𝑛) returns zero. the TYPE is set field SENSORD(𝑛, 𝑖𝑑𝑓𝑙𝑡) Returns the current value of *SENSOR_DEFINE sensor having ID 𝑛. Idflt is the optional filter ID defined using *DEFINE_- FILTER. Contact Force Functions: FUNCTION DESCRIPTION RCFORC(id, ims, comp, local) Returns the component comp of contact interface id as calculated in the local coordinate system local . If local equals zero then forces are reported in the global coordinate system. Forces are reported for the slave side when ims = 1 or master side when ims = 2. Following are the admissible values of comp and their corresponding force component. comp.EQ.1: 𝑥 force component comp.EQ.2: 𝑦 force component comp.EQ.3: 𝑧 force component comp.EQ.4: resultant force Element Specific Functions: FUNCTION DESCRIPTION BEAM(id, jflag, comp, rm) the comp force component Returns of beam id as calculated in the local coordinate system rm. Forces are reported in the global coordinate system if rm is zero. If rm equals -1 the beam’s 𝑟, 𝑠, and 𝑡 force/moment is returned. If jflag is set to zero FUNCTION DESCRIPTION then the force/torque acting on 𝑛1 end of the beam is returned, otherwise if jflag is set to 1 the force/torque on the 𝑛2 end of the beam is returned. See *ELEMENT_BEAM for the nodal connectivity rule defining 𝑛1 and 𝑛2. Admissible values of comp are 1-8 and correspond to the following components. comp.EQ.1: force magnitude comp.EQ.2: 𝑥 force (axial 𝑟-force, rm = -1) comp.EQ.3: 𝑦 force (𝑠-shear force, rm = -1) comp.EQ.4: 𝑧 force (𝑡-shear force, rm = -1) comp.EQ.5: torque magnitude comp.EQ.6: 𝑥 torque (torsion, rm = -1) comp.EQ.7: 𝑦 torque (𝑠-moment, rm = -1) comp.EQ.8: 𝑧 torque (𝑡-moment, rm = -1) ELHIST(eid, etype, comp, ipt, local) the elemental quantity comp Returns of element eid as calculated in the local coordinate system local. Quantities are reported in the global coordinate system if The parameter ipt specifies local is zero. for particular whether integration point or maximum, minimum, or averaging is applied across the integration points. the quantity is The following element classes, specified with etype, are supported. etype.EQ.0: solid etype.EQ.2: thin shell Following are admissible values of comp and the corresponding elemental quantity. comp.EQ.1: 𝑥 stress comp.EQ.2: 𝑦 stress comp.EQ.3: 𝑧 stress comp.EQ.4: 𝑥𝑦 stress FUNCTION DESCRIPTION comp.EQ.5: 𝑦𝑧 stress comp.EQ.6: 𝑧𝑥 stress comp.EQ.7: effective plastic strain comp.EQ.8: hydrostatic pressure comp.EQ.9: effective stress comp.EQ.11: 𝑥 strain comp.EQ.12: 𝑦 strain comp.EQ.13: 𝑧 strain comp.EQ.14: 𝑥𝑦 strain comp.EQ.15: 𝑦𝑧 strain comp.EQ.16: 𝑧𝑥 strain Integration point options, specified with ipt, follow. ipt.GE.1: quantity is reported for integration point number ipt ipt.EQ.-1: maximum of all integration points (default) ipt.EQ.-2: average of all integration points ipt.EQ.-3: minimum of all integration points ipt.EQ.-4: lower surface integration point ipt.EQ.-5: upper surface integration point ipt.EQ.-6: middle surface integration point local currently The local coordinate option defaults to the global coordinate system for solid elements and other coordinate system options are unavailable. In the case of thin shell elements the quantity is reported only in the element local coordinate system. local.EQ.1: global coordinate system (solid elements) local.EQ.2: element coordinate system (thin shell elements) FUNCTION DESCRIPTION JOINT(id, jflag, comp, rm) the comp force component Returns due to rigid body joint id as calculated in the local coordinate system rm. If jflag is set to zero then the force/torque acting on 𝑛1 end of the The force/torque on the 𝑛2 end of the joint is returned if See *CON- jflag is set to 1. STRAINED_JOINT for the rule defining n1 and 𝑛2. joint is returned. Admissible values of comp are 1-8 and correspond to the following components. comp.EQ.1: force magnitude comp.EQ.2: 𝑥 force comp.EQ.3: 𝑦 force comp.EQ.4: 𝑧 force comp.EQ.5: torque magnitude comp.EQ.6: 𝑥 torque comp.EQ.7: 𝑦 torque comp.EQ.8: 𝑧 torque Nodal Specific Functions: FUNCTION DESCRIPTION TEMP(𝑛) Returns the temperature of node 𝑛 General Functions FUNCTION DESCRIPTION CHEBY(𝑥, 𝑥0, 𝑎0, … , 𝑎30) Evaluates a Chebyshev polynomial at the user specified value 𝑥. The parameters 𝑥0, 𝑎0, 𝑎1, …, 𝑎30 are used the to define polynomial defined by: the constants for 𝐶(𝑥) = ∑ 𝑎𝑗𝑇𝑗(𝑥 − 𝑥0) where the functions 𝑇𝑗 is defined recursively as FUNCTION DESCRIPTION 𝑇𝑗(𝑥 − 𝑥0) = 2(𝑥 − 𝑥0)𝑇𝑗−1(𝑥 − 𝑥0) − 𝑇𝑗−2(𝑥 − 𝑥0) where 𝑇0(𝑥 − 𝑥0) = 1 𝑇1(𝑥 − 𝑥0) = 𝑥 − 𝑥0 Evaluates a Fourier cosine series at the user specified value x. The parameters x0, a0, a1, …, a30 are used to define the constants for the series defined by: 𝐹(𝑥) = ∑ 𝑎𝑗𝑇𝑗(𝑥 − 𝑥0) where 𝑇𝑗(𝑥 − 𝑥0) = cos[𝑗ω(𝑥 − 𝑥0)] Evaluates a Fourier sine series at the user specified value 𝑥. The parameters 𝑥0, 𝑎0, 𝑎1, …, 𝑎30 are used to define the constants for the series defined by: 𝐹(𝑥) = ∑ 𝑎𝑗𝑇𝑗(𝑥 − 𝑥0) where 𝑇𝑗(𝑥 − 𝑥0) = sin[𝑗ω(𝑥 − 𝑥0)] Arithmetic if conditional where 𝑎𝑖 can be a constant or any legal expression described in *DE- FINE_CURVE_FUNCTION. example, 𝑎1=’CX(100)’ sets the first argument to be the x- coordinate of node 100. {⎧the value of 𝑎2 the value of 𝑎3 ⎩{⎨ the value of 𝑎4 if the value of 𝑎1 < 0 if the value of 𝑎1 = 0 if the value of 𝑎1 > 0 IF = For Evaluates the control signal of a PID controller d𝑒(𝑡) d𝑡 𝑢(𝑡) = kp× 𝑒(𝑡) + ki× ∫ 𝑒(𝜏)𝑑𝜏 + kd× FORCOS(𝑥, 𝑥0, 𝜔[, 𝑎0, … , 𝑎30]) FORSIN(𝑥, 𝑥0, 𝜔[, 𝑎0, … , 𝑎30]) IF(𝑎1, 𝑎2, 𝑎3, 𝑎4) PIDCTL(meas, ref, kp, ki, kd, tf, ei0, sint, umin, umax) where 𝑒(𝑡) is the control error defined as the difference between the reference value ref and the measured value, meas 𝑒(𝑡) = ref− 𝑚𝑒𝑎𝑠 FUNCTION DESCRIPTION The control parameters are proportional gain kp, integral gain ki, derivative gain kd and low-pass filter tf for the derivative calculation d𝑒(𝑡𝑛) d𝑡 = d𝑒(𝑡𝑛−1) d𝑡 𝑡𝑓 ∆𝑡 + 𝑡𝑓 + ∆𝑡 ∆𝑡 + 𝑡𝑓 × 𝑒(𝑡𝑛) − 𝑒(𝑡𝑛−1) ∆𝑡 Ei0 is the initial integral value at time = 0. Sint is the sampling interval. Umin and umax, the lower and upper limit of a control signal, can be used to represent the saturation limits of an actuator. When the signal is not within the limits, it is clipped to the saturation limit, i.e., integration is skipped to avoid integrator wind-up. Input parameter can be a constant or any legal *DEFINE_CURVE_- expression described For example, meas=’CX(100)’ FUNCTION. measures the x-coordinate of node 100, ref =’LC200’ uses curve 200 as the reference value. in POLY(𝑥, 𝑥0, 𝑎0, … , 𝑎30) SHF(𝑥, 𝑥0, 𝑎, 𝜔[, 𝜙, 𝑏]) Evaluates a standard polynomial at the user specified value 𝑥. The parameters 𝑥0, 𝑎0, 𝑎1, …, 𝑎30 the to define are used polynomial defined by: the constants for 𝑃(𝑥) = 𝑎0 + 𝑎1(𝑥 − 𝑥0) + 𝑎2(𝑥 − 𝑥0)2 + ⋯ + 𝑎𝑛(𝑥 − 𝑥0)𝑛 Evaluates a Fourier sine series at the user specified value 𝑥. The parameters 𝑥0, 𝑎0, 𝑎1, …, 𝑎30 are used to define the constants for the series defined by: SHF = 𝑎sin[ω(𝑥 − 𝑥0) − ϕ] + 𝑏 STEP(𝑥, 𝑥0, ℎ0, 𝑥1, ℎ1) Approximates the Heaviside function with a cubic polynomial using the equation: STEP = ⎧ℎ0 { { ⎨ { { ⎩ ℎ1 ℎ0 + (ℎ1 − ℎ0) [ (𝑥 − 𝑥0) ] (𝑥1 − 𝑥0) {3 − 2 [ (𝑥 − 𝑥0) (𝑥1 − 𝑥0) if 𝑥 ≤ 𝑥0 ]} if 𝑥 < 𝑥 < 𝑥1 if 𝑥 ≥ 𝑥1 Electromagnetic solver (EM) Functions FUNCTION DESCRIPTION EM_ELHIST(iele, ifield, idir) Returns the elemental quantity of element iele in the global reference frame. EM_NDHIST(inode, ifield, idir) RM_PAHIST(ipart, ifield, idir) Returns the nodal quantity of node inode in the global reference frame. Returns the value integrated over the whole part given by ipart. ifield can be 7, 8 and 11 only. Admissible values of ifield are 1-10 and correspond to the following variables. comp.EQ.1: scalar potential comp.EQ.2: vector potential comp.EQ.3: electric field comp.EQ.4: 𝐁 field comp.EQ.5: 𝐇 field comp.EQ.6: current density comp.EQ.7: Lorentz force comp.EQ.8: current density comp.EQ.9: Lorentz force comp.EQ.10: relative permeability comp.EQ.11: magnetic energy (in the conductor only) Admissible values of idir are 1-4 and correspond to the following components. comp.EQ.1: 𝑥-component comp.EQ.2: 𝑦-component comp.EQ.3: 𝑧-component comp.EQ.4: Norm Remarks: 1. Local Coordinate Systems Required for Rotational Motion. A local coordinate system must be attached to nodes if they are referenced by functions involving rotational motion, for example, angular displacement or angular velocity. The local coordinate system is attached to the node using *DEFINE_- COORDINATE_NODES and FLAG=1 is a requirement. Furthermore, the three nodes which comprise the coordinate system must lie on the same body. Simi- larly, a local coordinate system must also be attached to node 𝑛3 if 𝑛3 is refer- enced in functions: DX, DY, DZ, VX, VY, VZ, WX, WY, WZ, ACCX, ACCY, ACCZ, WDTX, WDTY, WDTZ, FX, FY, FZ, TX, TY, or TZ. 2. Default is Radians. Unless otherwise noted units of radians are always used for the arguments and output of functions involving angular measures. 3. The following examples serve only as an illustration of syntax. Example 1: Define a curve 10 whose ordinate is, 𝑓 (𝑥) = (ordinate of load curve 9) × (magnitude of translation velocity at node 22)3. *DEFINE_CURVE_FUNCTION 10 0.5*lc9*vm(22)**3 Example 2: Define a curve 101 whose ordinate is, 𝑓 (𝑥) = −2(z translational displacement of node 38) × sin(20𝜋𝑡). *DEFINE_CURVE_FUNCTION 101 -2.*dz(38)*sin(2.*pi*10.*time) Example 3: Define a curve 202 whose ordinate is, 𝑓 (𝑥) = { cos(4𝜋𝑡) 𝑖𝑓 𝑡 ≤ 5. 0. 𝑖𝑓 𝑡 > 5. *DEFINE_CURVE_FUNCTION 202 If(TIME-5.,COS(4.*PI*TIME),COS(4.*PI*TIME),0.) *DEFINE Purpose: Define a smoothly varying curve using few parameters. This shape is useful for velocity control of tools in metal forming applications. Vmax Trise Trise dist = ∫v(t)dt 0.0 0.0 Tstart Simulation Time Tend Figure 15-17. Smooth curve created automatically using *DEFINE_CURVE_- SMOOTH. This shape is commonly used to control velocity of tools in metal forming applications as shown in the above graph, but can be used for other applications in place of any standard load curve. Card 1 2 3 4 5 6 7 8 Variable LCID SIDR DIST TSTART TEND TRISE VMAX Type I I F F F F F Default none none none none none none none VARIABLE DESCRIPTION LCID Load curve ID, must be unique. *DEFINE_CURVE_SMOOTH DESCRIPTION SIDR Stress initialization by dynamic relaxation: EQ.0: load curve used in transient analysis only or for other applications, EQ.1: load curve used in stress initialization but not transient analysis, EQ.2: load curve applies to both initialization and transient analysis. DIST Total distance tool will travel (area under curve). TSTART Time curve starts to rise TEND Time curve returns to zero. If TEND is nonzero, VMAX will be computed automatically to satisfy required travel distance DIST. Input either TEND or VMAX. TRISE Rise time VMAX Maximum velocity (maximum value of curve). If VMAX is nonzero, TEND will be computed automatically to satisfy required travel distance DIST. Input either TEND or VMAX. *DEFINE_CURVE_TRIM_{OPTION} Available options include: <BLANK> 3D NEW Purpose: This keyword is developed to define curves and controls for sheet blank trimming in sheet metal forming. It can also be used to define mesh adaptivity along a curve prior to the start of a simulation, using variable TCTOL and keyword *CON- TROL_ADAPTIVE_CURVE. When the option 3D is used, the trimming is processed based on the element normal rather than a vector. The option NEW is used to trim in a fixed direction specified by a vector, and is also called 2D trimming. Currently this keyword applies to: • 2D and 3D trimming of shell elements, • 2D and 3D trimming of solids, • 2D and 3D adaptive trimming of adaptive-meshed sandwiched parts (limit to a core of one layer of solid elements with outer layers of shell elements, see “IFSAND” under *CONTROL_ADAPTIVE), • 2D and 3D trimming of non-adaptive sandwiched parts (a core of multiple layers of solid elements with outer layers of shell elements), and, • 2D trimming of thick shell elements (TSHELL). This keyword is not applicable to axisymmetric solids or 2D plane strain/stress elements. Related keywords include *ELEMENT_TRIM, *CONTROL_FORMING_- TRIMMING, *CONTROL_ADAPTIVE_CURVE, *INCLUDE_TRIM, and *INCLUDE. Another closely related keyword is *CONTROL_FORMING_TRIM_MERGE, which automatically closes an open trim curve with a user-specified tolerance. Trimming of shell and solid elements are supported starting in LS-PrePost 4.0 and LS-PrePost 4.3, respectively, under Application → MetalForming → Easy Setup. Card 1 1 2 3 4 5 6 7 8 Variable TCID TCTYPE TFLG TDIR TCTOL TOLN / IGB NSEED1 NSEED2 Type I Default none I 1 I none I 0 F F I I 0.25 2.0 / 0 none none Remarks Fig. 15-18 Fig. 15-19 Point Cards. Additional cards for TCTYPE = 1. Put one point per card (2E20.0). Input is terminated at the next keyword (“*”) card. Card 2 1 2 3 4 5 6 7 8 Variable Type CX F Default 0.0 CY F 0.0 CZ F 0.0 IGES File Card. Additional card for TCTYPE = 2. Card 3 1 2 3 4 5 6 7 8 Variable Type FILENAME C VARIABLE DESCRIPTION TCID ID number for trim curve. VARIABLE DESCRIPTION TCTYPE Trim curve type: EQ.1: Curve data in XYZ following procedures outlined in Figures under *INTERFACE_- BLANKSIZE. In addition, only this format is allowed in *INTERFACE_COMPENSATION_NEW. format, obtained EQ.2: IGES trim curve. TFLG Element removal option (applies to option NEW only): EQ.-1: remove material outside curve; EQ.1: remove material inside curve. TDIR If the option NEW is used, this is the ID of a vector (*DEFINE_- VECTOR) giving the trim direction . EQ.0: default vector (0.0,0.0,1.0) is used. Curve is defined in global XY plane, and projected onto mesh in global Z- direction to define trim line. If the option 3D is used, TDIR is used to indicate whether the trim curve is near the top or bottom surface of the solids or laminates (>Revision 101964), see Trimming. EQ.1: trim curve is located near the top surface (default). EQ.-1: trim curve is located near the bottom surface. TCTOL Tolerance limiting size of small elements created during trimming . LT.0: "simple" trimming, producing jagged edge mesh When used together with *CONTROL_ADAPTIVE_CURVE, it is a distance from the curve out (both sides). Within this distance the blank mesh will be refined, as stated in remarks below. TOLN / IGB *DEFINE_CURVE_TRIM DESCRIPTION If the option 3D is used, TOLN represents the maximum gap between the trimming curve and the mesh. If the gap is bigger than this value, this section in the curve will not be used. If the option NEW is used, then the variable IGB is defined as follows: IGB.EQ.0: trimming curve is defined in local coordinate system. This is the default value. If this value is chosen for IGB, then the variable TDIR and the key- word *DEFINE_VECTOR need to be defined accord- ing to Figure 15-18. IGB.EQ.1: trimming curve is defined in global coordinate system. NSEED1/ NSEED2 A node ID on the blank in the area that remains after trimming, applicable to both options 3D or NEW. LT.0: positive number is a node ID, which may not necessarily be from the blank, referring to remarks below. CX, CY, CZ X, Y, Z-coordinate of trim curve. TCTYPE = 1. Define if and only if FILENAME Name of IGES database containing trim curve(s). Define if and only if TCTYPE = 2. Trimming capability summary: This keyword and its options deal with trimming of the following scenarios: 2D (along one direction) 3D (element normal) 2D & 3D Double Trim Adaptive mesh Shell Solids Yes Yes Yes Yes Yes Yes Yes N/A Laminates Yes Yes Yes One layer of solids only; Multiple layers of solids okay for non-adaptive mesh. TSHELL Yes N/A N/A N/A About the options and trim curves: The option NEW activates a new searching algorithm, which enables a much faster trimming operation compared with option 3D. For big models, the improvement in computational efficiency of the NEW option is significant. In addition, users are required to pick a seed node (or position coordinates), as is the case with the 3D option. Both options are now available under the “Trimming” feature of LS-PrePost 4.0’s eZ- Setup for metal forming application (http://ftp.lstc.com/anonymous/outgoing/- lsprepost/4.0/metalforming/). Only IGES entities 110 and 106 are supported when using the TCTYPE of 2. The eZ-Setup for trimming function ensures correct IGES files are written for trimming simulation. For the option NEW, Revision 68643 and later releases enable trimming of a part where trim lines go beyond the part boundary. This is illustrated in Figure 15-24. Enclosed trimming curves (same start and end points) are required for all options. Furthermore, for each enclosed trimming curve, only one curve segment is acceptable for the option 3D; while several curve segments are acceptable with the option NEW. Curves can be manipulated through the use of Merge and break features in LS-PrePost4.0, found under Curve/Merge (always select piecewise under Merge) and break. In case of 3D trimming, trim curves need to be sufficiently close to the part. A feature of curve projection to the mesh in LS-PrePost can be used to process the trim curves. The feature is accessible under GeoTol/Project/Closest Proj/Project to Element/By Part. Double precision LS-DYNA executable may also help in this situation. Choice of 2D or 3D trimming depends on the to-be-trimmed part geometry. 2D trimming can be used if trimming is to be done on the relatively flat area of the part, while 3D trimming must be selected for trimming on a inclined or vertical draw wall area for precise trimming. Seed node definition: This keyword in combination with *ELEMENT_TRIM trims the requested parts before a job starts (pre-trimming), and can handle adaptive mesh. If the keyword *ELEMENT_- TRIM does not exist the parts are trimmed after the job is terminated (post-trimming). Seed node is used to define which side of the drawn panel to be kept after the trimming. With the frequent application of adaptive re-meshing, the seed node for trimming is often unknown until the draw forming is complete. With the negative NSEED variable, an extra node unrelated to the blank and tools can be created for the definition of the seed node, enabling trimming process independent of the previous process simulation results. The extra node can be defined using keyword *NODE. A partial keyword input example for the trimming of a double-attached NUMISHEET2002 fender outer with the option NEW is listed below, where a 2D trimming is performed with IGES file doubletrim.iges in the global Z-axis, with two nodes of negative ID 43356 and 18764 assigned to the variables NSEED1 and NSEED2, respectively. The two seed nodes are defined off the stationary lower post, and do not necessarily need to be a part of the post, as shown in Figure 15-20. The drawn panels in wire frame are shown in Figure 15-21, along with the thickness/thinning contour (Figure 15-22). In Figure 15-23, the drawn panels are trimmed and separated. *KEYWORD *CONTROL_TERMINATION 0.000 *CONTROL_SHELL ...... *CONTROL_OUTPUT ...... *DATABASE_BINARY_D3PLOT ...... *DATABASE_EXTENT_BINARY ...... $---+----1----+----2----+----3----+----4----+----5----+----6----+----7----+----8 *SET_PART_LIST ...... *PART Blank ...... *SECTION_SHELL ...... *MAT_3-PARAMETER_BARLAT ...... $---+----1----+----2----+----3----+----4----+----5----+----6----+----7----+----8 *INCLUDE_TRIM drawn.dynain *ELEMENT_TRIM 1 *DEFINE_CURVE_TRIM_NEW $# TCID TCTYPE TFLG TDIR TCTOL TOLN NSEED1 NSEED2 1 2 0 0.250 1 -43356 -18764 doubletrim.iges $---+----1----+----2----+----3----+----4----+----5----+----6----+----7----+----8 *NODE 18764,-184.565,84.755,78.392 43356,-1038.41,119.154,78.375 *INTERFACE_SPRINGBACK_LSDYNA ...... *END If the seed node is too far away from the blank it will be projected to the blank and the new position will be used as the seed node. Typically, this node can be selected from the stationary tool in its home position. Alternatively, if the variable NSEEDs are not defined, the seeds can be defined using *DEFINE_TRIM_SEED_POINT_COORDINATES. A partial keyword input is provided below for trimming of the same double-attached fender outer. *INCLUDE_TRIM drawn.dynain *ELEMENT_TRIM 1 *DEFINE_CURVE_TRIM_NEW $# TCID TCTYPE TFLG TDIR TCTOL TOLN NSEED1 NSEED2 1 2 0 0.250 1 doubletrim.iges *DEFINE_TRIM_SEED_POINT_COORDINATES $ NSEED X1 Y1 Z1 X2 Y2 Z2 2 -184.565 84.755 78.392 -1038.41 119.154 78.375 Again, selecting a seed node is quite easy in “Trimming” process of LS-PrePost4.0 eZSetup for metal forming application. General adaptive re-meshing and element fixing during trimming: In case of large element size along the trim curves, the blank mesh can be pre-adapted along the trim curves before trimming by adding the keyword *CONTROL_ADAP- TIVE_CURVE to the above example for a better quality trim edge. The following indicates refining meshes for part set ID 1 no more than three levels along the trim curves, or until element size reaches 3.0: Care should be taken since too small of the value SMIN and too large value of N could result in excessive amount of elements to be generated. *CONTROL_ADAPTIVE_CURVE $# IDSET ITYPE N SMIN ITRIOPT 1 2 3 3.0 0 Sometimes it is helpful to conduct a check of the trimmed mesh along the edge in the same trimming input deck using the keyword *CONTROL_CHECK_SHELL. This is especially useful for the next continued process simulation. For detailed usage, check for an updated remarks for the keyword. The trimming tolerance TCTOL limits the size of the smallest element created during trimming. A value of 0.0 places no limit on element size. A value of 0.5 restricts new elements to be at least half of the size of the parent element. A value of 1.0 allows no new elements to be generated, only repositioning of existing nodes to lie on the trim curve. A negative tolerance value activates "simple" trimming, where entire elements are removed, leaving a jagged edge. TCTOL used as mesh refinement width along a curve: The variable TCTOL can be used to control the mesh refinement along a curve when used together with *CONTROL_ADAPTIVE_CURVE. In this scenario, it is the distance from both sides of the curve within which the mesh will be refined. The mesh will be refined in the beginning of the simulation. This method offers greater control on the number of elements to be generated during mesh refinement, as compared to that without using this variable. A detailed description and example is provided under the manual section under *CONTROL_ADAPTIVE_CURVE. The keyword *INCLUDE_TRIM is recommended to be used at all times, either for trimming or for mesh refinement purpose, except in case where to-be-trimmed sheet blank has no stress and strain information (no *INITIAL_STRESS_SHELL, and *INI- TIAL_STRAIN_SHELL cards present in the sheet blank keyword or dynain file), the keyword *INCLUDE must be used. A check box to indicate that the blank is free of stress and strain information is provided in the “Trimming” process in the eZ-Setup for users to set up a trimming input deck under the circumstance. 2D and 3D trimming of solid elements and laminates: Trimming curve preparation, file inclusion, etc. The requirement for trimming curves definition of solids in case of 3D trimming is different from that of shell trimming. The trim curve should be created based on solid element normal. If trim curve is created closer to the top surface, the variable TDIR should be set to 1; if closer to the bottom surface, set to -1, see Figure 15-27. Normal directions of solid elements can be viewed using LS-PrePost starting in version 4.2 with the menu option of EleTol → Normal → Entity Type: Solid → By Part, and set a large V-Size. In addition, when defining a trim curve for the 3D trimming of both solids and laminates, the curve should be as close to either the top or bottom side of the part as possible to enable a successful trimming. This is especially true if wrinkles are present in the panels to be trimmed. LS-PrePost can be used to project the curves to the part, via menu option: GeoTol → Project → Closest proj → Project to Element. Either top or bottom side of the part can be selected as “Element” by part. The curves may need to be refined with more points before projection, using menu option: Curves → Method: Respace → By number. Sufficient number of points may be entered to capture the sheet metal surface contour. For solid element trimming, only *INCLUDE_TRIM (not *INCLUDE) is supported to include the dynain file from a previous process (for example, forming) simulation. 2D trimming of solid elements As of Revision 92088, 2D (option NEW) trimming in any direction (defined by a vector) of solid elements is available. An illustration of the 2D trim is shown in Figure 15-25. A partial keyword example is provided below, where trim curves trimcurves2d.iges is being used to perform a solid element trimming along a vector defined along the global Z-axis. *KEYWORD *INCLUDE_TRIM incoming.dynain $---+----1----+----2----+----3----+----4----+----5----+----6----+----7----+----8 *PARAMETER_EXPRESSION ... *CONTROL_TERMINATION $ ENDTIM 0.0 *CONTROL_OUTPUT ... *DATABASE_XXX ... *PART Solid Blank $# pid secid mid &blk1pid &blk1sec &blk1mid *SECTION_Solid &blk1sec,&elform *MAT_PIECEWISE_LINEAR_PLASTICITY ... $---+----1----+----2----+----3----+----4----+----5----+----6----+----7----+----8 $ Trim cards $---+----1----+----2----+----3----+----4----+----5----+----6----+----7----+----8 *CONTROL_FORMING_TRIMMING $ PSID &blksid *DEFINE_TRIM_SEED_POINT_COORDINATES $ NSEED,X1,Y1,Z1,X2,Y2,Z2 1,&seedx,&seedy,&seedz $---+----1----+----2----+----3----+----4----+----5----+----6----+----7----+----8 *DEFINE_CURVE_TRIM_NEW $# tcid tctype tflg tdir tctol toln nseed1 nseed2 2 2 0 1 0.10000 1.000000 0 0 $# filename trimcurves2d.iges *DEFINE_VECTOR $# vid xt yt zt xh yh zh cid 1 0.000 0.000 0.000 0.000 0.000 1.000000 0 *INTERFACE_SPRINGBACK_LSDYNA $ PSID &blksid,&nshv *END Currently, 2D trimming of solids in some cases may be approximate. The trimming will trim the top and bottom sides of the elements, not crossing over to the other sides. This can be seen, for instance, trimming involving a radius. 3D (normal) trimming of solid elements As of Revision 93467 3D trimming (option 3D) of solid elements is available. From the previous input, in case of 3D trimming, the option NEW is changed to 3D, and trim curves trimcurves3d.iges is used. In the example below, the variable TDIR is set to “1” since the trim curve is on the positive side of the element normal (Figure 15-27). Since 3D trimming are along the element normal directions, *DEFINE_VECTOR card is no longer needed. *DEFINE_CURVE_TRIM_3D $# tcid tctype tflg tdir tctol toln nseed1 nseed2 2 2 0 1 0.10000 1.000000 0 0 $# filename trimcurves3d.iges Again, the projection of trim curves onto either the top or bottom surface of the blank is important to ensure a smooth and successful trimming. 2D and 3D trimming of non-adaptive-meshed sandwiched parts (laminates) 2D and 3D trimming of non-adaptive-meshed laminates are available starting in Revision 92289. Trimming of the laminates can have multiple layers of solid elements, sandwiched by a top and a bottom layer of shell elements. Note that the nodes of shell elements must share the nodes with solid elements at the top and bottom layers. An illustration of the trim is shown in Figure 15-26. The input deck is similar to those used for trimming of solid elements, except the variable ITYP under *CONTROL_FORM- ING_TRIMMING should be set to “1” to activate the trimming of laminates in both 2D and 3D conditions: *CONTROL_FORMING_TRIMMING $---+----1----+----2----+----3----+----4----+----5----+----6----+----7----+----8 $ PSID ITYP &blksid 1 Again, in the case of 3D trimming, the projection of trim curves onto either the top or bottom surface of the blank is important to ensure a smooth and successful trim. 2D and 3D trimming of adaptive-meshed sandwiched parts (laminates) 2D and 3D trimming of adaptive-meshed laminates are available starting in Revision 108770. Trimming of the laminates is limited to one core layer of solid elements, sandwiched by a top and a bottom layer of shell elements. Shell elements share the same nodes as the solid elements. the cut by Note elements are refined automatically along the trim curves until no slave nodes would be the keyword curves. *CONTROL_ADAPTIVE_CURVE must not be used, since it is only applied to shell elements, and would cause error termination otherwise. Furthermore, unlike the mesh refinement along the trim curve during shell element trimming, this trimming requires no additional adaptivity-related keyword inputs. An example of the trimming on the 2005 NUMISHEET Cross Member is shown in Figure 15-28. addition, trim In Again, in the case of 3D trimming, the projection of trim curves onto either the top or bottom surface of the blank is important to ensure a smooth and successful trim. Summary – trimming of solids and laminates In summary, the trimming input files between solids/laminates and shells are different in a few ways. For solids, *SECTION_SOLID is needed in place of *SECTION_SHELL. For laminates, in addition to setting the ITYP = 1 in *CONTROL_FORMING_TRIM- MING, both *SECTION_SHELL and *SECTION_SOLID need to be defined. The position of a trim curve for 3D trimming of solids needs to be defined according to Figure 15-27. Adaptive-meshed sandwiched parts (limit to a core of one layer of solid elements with outer layers of shell elements) can be 2D or 3D trimmed with adaptive mesh refinement along the trim curves. Non-adaptive-meshed sandwiched parts (a core of multiple layers of solid elements with outer layers of shell elements) can be 2D and 3D trimmed. In all trimming of solids and laminates, only dynain file is written out (no d3plot files will be output), and finally, *INCLUDE_TRIM is to be used. In the case of 3D trimming, the projection of trim curves onto either the top or bottom surface of the blank is important to ensure a smooth and successful trim. 2D trimming of thick shell elements (TSHELL): 2D trimming of TSHELL is supported starting from Revision 107957. Note by definition, TSHELL has only one layer of solid elements, and is defined by keyword *SECTION_TSHELL. Note also *INCLUDE_TRIM (not *INCLUDE) must be used to include the dynain file to be trimmed. Input deck for 2D trimming of TSHELL is similar to what is used for trimming of solid elements. 2D and 3D trimming of double-attached solids and laminates: These features are available starting in Revision 110140. Both seed point coordinates can be specified in *DEFINE_TRIM_SEED_POINT_COORDINATES to define a seed coordinate for each part, as shown below: *DEFINE_TRIM_SEED_POINT_COORDINATES $ NSEED X1 Y1 Z1 X2 Y2 Z2 2 -184.565 84.755 78.392 -1038.41 119.154 78.375 In Figure 15-29, a 2D double-trimming example on a sandwiched part is shown using the 2005 NUMISHEET cross member. Two trim curves, two seed nodes are defined for each to be trimmed portion. The coordinates for seed node #1 is (-184.565, 84.755, 78.392) and is (-1038.41, 119.154, 78.375) for seed node #2. Trimmed results are satisfactory. Revision information: Revision information are as follows: 1. Revision 54608 and 52312: negative seed node option is available for the options 3D and NEW, respectively. 2. Revision 65630: Use of TCTOL as a distance for mesh refinement (when used together with *CONTROL_ADAPTIVE_CURVE) is available. 3. Revision 68643: trimming is enabled for those trim lines going beyond the part boundary. 4. Revision 92088: 2D (option NEW) trimming of solid elements. 5. Revision 92289: 2D and 3-D (option 3D) trimming of laminates. 6. Revision 93467: 3D trimming of solid elements. 7. Revision 101964: TDIR definition activated for 3D trimming of top and bottom surfaces of solid elements and laminates. 8. Revision 107957: 2D trimming of TSHELL. 9. Revision 109047: 2D and 3D trimming of adaptive-meshed sandwiched part. 10. Revision 110140: 2D and 3D trimming of solids and laminates of double- attached parts. 11. Latter Revisions may incorporate more improvements and are suggested to be used for trimming. Part to be trimmed Trim curve (local system) Trim curve (projected) Figure 15-18. Trimming Orientation Vector. The tail (T) and head (H) points define a local coordinate system (x,y,z). The global coordinate system is named (X,Y,Z). The local x-direction is constructed in the Xz plane. If X and z nearly coincide (|X • z| > 0.95), then the local x-direction is instead constructed in the Yz plane. Trim curve data is input in the x-y plane, and projected in the z-direction onto the deformed mesh to obtain the trim line. Tol = 0.25 (default) Tol = 0.01 Figure 15-19. Trimming Tolerance. The tolerance limits the size of the small elements generated during trimming. The default tolerance (left) produces large elements. Using a tolerance of 0.01 (right) allows smaller elements, and more detail in the trim line. Seed nodes Trim line 18764 43356 Punch opening line Figure 15-20. Trimming of a double-attached part (NUMISHEET2002 Fender Outer). Blank edge line Punch opening line Figure 15-21. The fender outer (draw complete) in wireframe mode. Figure 15-22. The fender outer - thickness/thinning plot on the drawn panel. Figure 15-23. The fender outer trim complete using the NSEED1/NSEED2 feature. Blank edge outline Trim line loops outside of the part periphery Punch opening line Figure 15-24. Revision 68643 deals with trim curves going beyond part boundary. Trim curves in red Three layers of solid elements through the thickness Trim vectors Figure 15-25. 2-D trimming of solids using *DEFINE_CURVE_TRIM_NEW Top layer of shell elements Five-layers of 3-D solid elements Trim curves (piecewise) Bottom layer of shell elements Figure 15-26. 3-D trimming of laminates (a core of multiple-layers of solid elements with shell elements) using *DEFINE_CURVE_TRIM_3D. Note that shell elements must share the same nodes with the solid elements at the top and bottom layer. top and bottom layers of Positive side of solid element normals; check solid normals using LS-PrePost4.2 Trim curve All solid element normals must be consistent. If trim curve is close to the positive normal side, set TDIR=1; otherwise set TDIR=-1. Respacing the curve with more points, project the respaced curve to the top or bottom solid surface may help the trimming. Figure 15-27. Define trim curve for 3D trimming of solid and laminates. Inner trim curve Outer trim curve Elements (both shells and solids) are automatically refined along the trim curves Mesh prior to trim Trimmed mesh Trim curves Drawn Panel 2005 NUMISHEET Cross Member - Drawn Panel and Trim Curves Figure 15-28. Trimming of an adaptive mesh on a sandwiched part. Meshes are automatically refined along the trim curves. Note that only one layer of solid element as a core is allowed for adaptive-meshed sandwich parts. Also top and bottom layer of shells must share the same nodes as the solid elements. The keyword *CONTROL_ADAPTIVE_CURVE must not be used. Trim curve #1 Drawn Panel Trimmed piece #1 *DEFINE Trim direction: global Z Trim curve #2 Seed node #2 Trimmed piece #2 Trim curves, seed nodes and direction defintion Trimmed results Figure 15-29. An example of 2D trimming of sandwiched part (laminates) from 2005 NUMISHEET benchmark - cross member. *DEFINE_DEATH_TIMES_OPTION Available options include: NODES SET RIGID Purpose: To dynamically define the death times for *BOUNDARY_PRESCRIBED_MO- TION based on the locations of nodes and rigid bodies. Once a node or rigid body moves past a plane or a geometric entity, the death time is set to the current time. The input in this section continues until the next ‘*’ card is detected. 5 6 7 8 Card 1 1 Variable GEO Type I Default Card 2 1 2 N1 I 0 2 3 N2 I 0 3 4 N3 I 0 4 5 6 Variable X_T Y_T Z_T X_H Y_H Z_H Type F F F F F F Default 7 R F 8 FLAG 1 ID Cards. Set the list of nodes and rigid bodies affected by this keyword. This input terminates at the next keyword (“*”) card. Card 3 1 2 3 4 5 6 7 8 Variable NSID1 NSID2 NSID3 NSID4 NSID5 NSID6 NSID7 NSID8 Type I I I I I I I GEO = 1 GEO = 3 GEO = 2 O = origin = X_T, Y_T, Z_T or coordinates of N1 V = X_H - X_T, Y_H - Y_T, Z_H - Z_T or coordinates of N3 - coordinates of N2 Figure 15-30. Geometry types. VARIABLE DESCRIPTION GEO Geometric entity type. = 1 plane, = 2 infinite cylinder, = 3 sphere N1 N2 N3 X_T Y_T Z_T X_H Y_H Z_H R Node defining the origin of the geometric entity (optional). Node defining the tail of the orientation vector (optional). Node defining the head of the orientation vector (optional). X coordinate of the origin of the geometric entity and the tail of the orientation vector. Y coordinate of the origin of the geometric entity and the tail of the orientation vector. Z coordinate of the origin of the geometric entity and the tail of the orientation vector. X coordinate of the head of the orientation vector. Y coordinate of the head of the orientation vector. Z coordinate of the head of the orientation vector. Radius of cylinder or sphere. FLAG *DEFINE_DEATH_TIMES DESCRIPTION +1 for killing motion when the node is outside of the geometric entity or on the positive side of the plane as defined by the normal direction, or -1 for the inside. NSIDi i-th node, node set, or rigid body Remarks: 1. Either N1 or X_T, Y_T, and Z_T should be specified, but not both. 2. Either N2 and N3 or X_H, Y_H, and Z_H should be specified, but not both. If N2 and N3. Specifying N2 and N3 is equivalent of setting the head of the vec- tor equal to the tail of the vector (X_T, Y_T, and Z_T) plus the vector from N2 to N3. *DEFINE Purpose: To define an interested region for Discrete Elements (DE) for high efficiency collision pair searching. Any DE leaving this domain will not be considered in the future DE searching and also disabled in the contact algorithm. 6 7 8 Card 1 Variable 1 ID 2 3 TYPE Xm Type I Default none I 0 F 0. 4 Ym F 0. 5 Zm F 0. VARIABLE DESCRIPTION ID TYPE Set ID/Box ID EQ.0: Part set ID EQ.1: Box ID Xm, Ym, Zm Factor for region's margin on each direction based on region length. The static coordinates limits are determined either by part set or box option. To extended those limits to provide a buffer zone, these factors can be used. The margin in each direction is calculated in the following way: Let 𝑋max and 𝑋min be the limits in the x direction. Then, Then the margin is computed from the input as, Δ𝑋 = 𝑋max − 𝑋min 𝑋margin = Xm × Δ𝑋 Then the corresponding limits for the active region are, 𝑋max ′ = 𝑋max + 𝑋margin ′ = 𝑋min − 𝑋margin 𝑋min *DEFINE_DE_BOND Purpose: To define a bond model for discrete element sphere (DES). Card 1 1 2 3 4 5 6 7 8 Variable SID STYPE BDFORM Type I Default none I 0 I 1 VARIABLE DESCRIPTION SID DES nodes STYPE EQ.0: DES node set EQ.1: DES node EQ.2: DES part set EQ.3: DES part BDFORM Bond formulation: EQ.1: Linear bond formulation. Card 2 for BDFORM = 1. Card 2 1 2 3 4 5 6 7 8 Variable PBN PBS PBN_S PBS_S SFA ALPHA MAXGA P Type F F F F F F F Default none none none none 1.0 0.0 1.E-4 VARIABLE DESCRIPTION PBN Parallel-bond modulus [Pa]. See Remark 1 VARIABLE DESCRIPTION PBS PBN_S PBS_S Parallel-bond stiffness ratio. shear stiffness/normal stiffness. See Remark 2 Parallel-bond maximum normal stress. A zero value defines an infinite maximum normal stress. Parallel-bond maximum shear stress. A zero value defines an infinite maximum shear stress. SFA Bond radius multiplier ALPHA Numerical damping MAXGAP Maximum gap between two bonded spheres GT.0.0: defines the ratio of the smaller radius of two bonded MAXGAP × spheres as the maximum gap, i.e. min(r1,r2) LT.0.0: absolute value is used as the maximum gap. Remarks: 1.The normal force is calculated as × A × ∆𝑢𝑛 ∆𝑓n = 𝑃𝐵𝑁 (𝑟0 + 𝑟1) where 2 𝐴 = 𝜋𝑟𝑒𝑓𝑓 𝑟𝑒𝑓𝑓 = 𝑚𝑖𝑛(𝑟0, 𝑟1) × 𝑆𝐹𝐴 2.The shear force is calculated as ∆𝑓s = PBS × 𝑃𝐵𝑁 (𝑟0 + 𝑟1) × A × ∆𝑢𝑠 *DEFINE_DE_BY_PART Purpose: To define control parameters for discrete element sphere by part ID. This card overrides the values set in *CONTROL_DISCRETE_ELEMENT. Card 1 1 2 3 4 5 6 7 8 Variable PID NDAMP TDAMP FRICS FRICR NORMK SHEARK Type I Default none Card 2 1 F 0 2 F 0 3 F 0 4 F 0 5 F F 0.01 2/7 6 7 8 Variable GAMMA VOL ANG Type Default F 0 F 0 F 0 Card 3 is optional Card 3 1 2 3 4 5 6 7 8 Variable LNORM LSHEAR FRICD DC Type Default I 0 I 0 VARIABLE F FRICS F 0 DESCRIPTION PID Part ID of DES nodes NDAMP Normal damping coefficient TDAMP Tangential damping coefficient DESCRIPTION VARIABLE FRICS Static coefficient of friction. The frictional coefficient is assumed to be dependent on the relative velocity 𝑣𝑟𝑒𝑙of the two DEM in contact 𝜇𝑐 = 𝐹𝑅𝐼𝐶𝐷 + (𝐹𝑅𝐼𝐶𝑆 − 𝐹𝑅𝐼𝐶𝐷)𝑒−𝐷𝐶∙∣𝑣𝑟𝑒𝑙∣. EQ.0: 3 DOF NE.0: 6 DOF (consider rotational DOF) FRICR Rolling friction coefficient NORMK Optional: scale factor of normal spring constant (Default = 0.01) SHEARK Optional: ratio between ShearK/NormK (Default = 2/7) GAMMA Liquid surface tension VOL ANG LNORM LSHEAR FRICD Volume fraction Contact angle Load curve ID of a curve that defines function for normal stiffness with respect to norm penetration ratio Load curve ID of a curve that defines function for shear stiffness with respect to norm penetration ratio Dynamic coefficient of friction. By default, FRICD = FRICS. The frictional coefficient is assumed to be dependent on the relative velocity 𝑣𝑟𝑒𝑙of the two DEM in contact 𝜇𝑐 = 𝐹𝑅𝐼𝐶𝐷 + (𝐹𝑅𝐼𝐶𝑆 − 𝐹𝑅𝐼𝐶𝐷)𝑒−𝐷𝐶∙∣𝑣𝑟𝑒𝑙∣. DC Exponential decay coefficient. The frictional coefficient is assumed to be dependent on the relative velocity 𝑣𝑟𝑒𝑙of the two DEM in contact 𝜇𝑐 = 𝐹𝑅𝐼𝐶𝐷 + (𝐹𝑅𝐼𝐶𝑆 − 𝐹𝑅𝐼𝐶𝐷)𝑒−𝐷𝐶∙∣𝑣𝑟𝑒𝑙∣. See also *CONTROL_DISCRETE_ELEMENT. *DEFINE_DE_HBOND Purpose: To define a heterogeneous bond model for discrete element sphere (DES). Card 1 1 2 3 4 5 6 7 8 Variable SID STYPE HBDFM IDIM Type I Default none I 0 I 1 I 3 VARIABLE DESCRIPTION SID DES nodes STYPE EQ.0: DES node set EQ.1: DES node EQ.2: DES part set EQ.3: DES part HBDFM Bond formulation: EQ.1: (Reserved) EQ.2: Nonlinear heterogeneous bond formulation for fracture analysis based on the general material models defined in the material cards. DES elements with different material models can be defined within one bond. IDIM Space dimension for DES bonds: EQ.2: for 2D plane strain problems EQ.3: for 3D problems. *DEFINE Card 1 2 3 4 5 6 7 8 Variable PBK_SF PBS_SF FRGK FRGS BONDR ALPHA DMG FRMDL Type F F F F F F F Default 1.0 1.0 none none none 0.0 1.0 I 1 VARIABLE DESCRIPTION PBK_SF Scale factor for volumetric stiffness of the bond. PBS_SF Scale factor for shear stiffness of the bond. FRGK Critical fracture energy release rate for volumetric deformation due to the hydrostatic pressure. Special Cases: EQ.0: A zero value specifies an infinite energy release rate for unbreakable bonds. LT.0: A negative value defines the energy release rate under volumetric compression (i.e. positive pressure) and FRGS defined below is used under volumetric expansion (i.e. negative pressure). FRGS Critical fracture energy release rate for shear deformation. Special Cases: EQ.0: A zero value specifies an infinite energy release rate for unbreakable bonds. FRGK.LT.0: See description for FRGK BONDR Influence radius of the DES nodes. ALPHA Numerical damping *DEFINE_DE_HBOND DESCRIPTION DMG Continuous parameter for damage model. EQ.1.0: The bond breaks if the fracture energy in the bond reaches the critical value. Microdamage is not calcu- lated. ∈ (0.5,1): Microdamage effects being once the fracture energy reaches DMG × FMG[K,S]. Upon the onset of micro- damage, the computed damage ratio will increase (monotonically) as the fracture energy grows. Bond weakening from microdamage is modeled by reduc- ing the bond stiffness in proportion to the damage ra- tio. FRMDL Fracture model: EQ.1: Fracture energy of shear deformation is calculated based on deviatoric stresses. EQ.2: Fracture energy of shear deformation is calculated based on deviatoric stresses, excluding the axial compo- nent (along the bond). EQ.3,4: Same as 1&2, respectively, but FRGK and FRGS are read as the total failure energy density and will be con- verted to the corresponding critical fracture energy re- lease rate. The total failure energy density is calculated as the total area under uniaxial tension stress-strain curve. EQ.5,6: Same as 3&4, respectively, as FRGK and FRGS are read as the total failure energy density but will not be con- verted. Instead, the failure energy within the bond will be calculated. Models 1&2 are more suitable for brittle materials, and Models 5&6 are easier for ductile materials. Models 3&4 can be used for moderately ductile fracture accordingly. This is the default fracture model and applied to all DES parts, even if they have different material models. More fracture models can be defined for different materials by specifying an interface ID (ITFID) in the optional card. Pre-crack Card. This card is optional. Optional 1 2 3 4 5 6 7 8 Variable PRECRK CKTYPE ITFID Type I Default none I 0 I 0 VARIABLE DESCRIPTION PRECRK Shell set, define 3D surfaces of the pre-crack CKTYPE ITFID EQ.0: Part set EQ.1: Part ID of the interface *INTERFACE_DE_HBOND, which defines different failure models for the heterogeneous bonds within each part and between two parts respectively. *DEFINE_DE_INJECTION_{OPTION} Available options include: <BLANK> ELLIPSE Purpose: This keyword injects discrete element spheres (DES) from specified a region at a flow rate given by a user defined curve. When the option is blank the region from which the DES emanate is assumed rectangular. The elliptical option indicates that the region is to be elliptical. Card 1 1 Variable PID 2 SID Type I I 3 XC F 4 YC F 5 ZC F 6 XL F 7 YL F Default none none 0.0 0.0 0.0 0.0 0.0 Card 2 1 2 3 4 Variable RMASS RMIN RMAX_S VX Type F F F F 5 VY F 6 VZ F 7 TBEG TEND F F Default none none RMIN 0.0 0.0 0.0 0.0 1020 Optional card. Card 3 1 2 3 4 5 6 7 8 Variable IFUNC Type Default I 0 15-140 (DEFINE) LS-DYNA R10.0 8 CID VARIABLE DESCRIPTION PID SID Part ID of new generated DES nodes Nodes and DES properties are generated Node set ID. automatically during input phase based on the user input and assigned to this SID. XC, YC, ZC 𝑥, 𝑦, 𝑧 coordinate of the center of injection plane XL YL CID For rectangular planes XL specifies the planar length along the 𝑥- axis in the coordinate system specified by CID. For elliptical planes XL specifies the length of the major axis. For rectangular planes YL specifies the planar length along the 𝑦- axis in the coordinate system specified by CID. For elliptical planes YL specifies the length of the minor axis. Optional local coordinate system ID, see *DEFINE_COORDI- NATE_SYSTEM RMASS Mass flow rate LT.0: Curve ID RMIN Minimum DES radius RMAX Maximum DES radius VX, VY, VZ Vector components defining the initial velocity of injected DES specified relative the coordinate system defined by CID. Birth time Death time EQ.0: Uniform distribution(Default) EQ.1: Gaussian distribution (Remark 1) TBEG TEND IFUNC Remarks: The distribution of particle radius follows Gaussian distribution 𝑓 (𝑟∣𝑟0, 𝜎) = − (𝑟−𝑟0)2 2𝜎 2 𝜎√2𝜋 Where the mean radius is given by and the standard deviation is 𝑟0 = 𝜎 = (𝑟max + 𝑟min), (𝑟max − 𝑟min) *DEFINE Purpose: To measure DES mass flow rate across a defined plane. See also the accompanying keyword *DATABASE_DEMASSFLOW which controls the output frequency. Card 1 1 2 3 4 5 6 7 8 Variable SLAVE MASTER STYPE MTYPE Type Default I 0 I 0 I 0 I 0 VARIABLE SLAVE DESCRIPTION Node set ID, node ID, part set ID or part ID defining DES on slave side. STYPE below indicates the ID type specified by SLAVE. MASTER Part set ID or part ID defining master surface. MTYPE below indicates the ID type specified by MASTER. STYPE Slave type. EQ.0: Slave node set EQ.1: Slave node EQ.2: Slave part set EQ.3: Slave part MTYPE Master type. EQ.0: Part set EQ.1: Part *DEFINE_DE_TO_BEAM_COUPLING Purpose: To define coupling interface between discrete element sphere (DES) and beam. Card 1 1 2 3 4 5 6 7 8 Variable SLAVE MASTER STYPE MTYPE Type Default I 0 Card 2 1 I 0 2 I 0 3 I 0 4 Variable FricS FricD DAMP BSORT Type Default F 0 F 0 F 0 I 100 5 6 7 8 VARIABLE DESCRIPTION SLAVE DES nodes MASTER Shell set STYPE MTYPE FricS FricD EQ.0: Slave node set EQ.1: Slave node EQ.2: Slave part set EQ.3: Slave part EQ.0: Part set EQ.1: Part Friction coefficient Rolling friction coefficient VARIABLE DESCRIPTION DAMP Damping coefficient BSORT Number of cycle between bucket sortings. (Default = 100) *DEFINE_DE_TO_SURFACE_COUPLING Purpose: To define a non-tied coupling interface between discrete element spheres (DES) and a surface defined by shell part(s) or solid part(s). This coupling is currently not implemented for tshell part(s). Card 1 1 2 3 4 5 6 7 8 Variable SLAVE MASTER STYPE MTYPE Type Default I 0 Card 2 1 I 0 2 I 0 3 I 0 4 5 6 7 8 Variable FricS FricD DAMP BSORT LCVx LCVy LCVz WEARC Type Default F 0 F 0 F 0 I 100 I 0 I 0 I 0 User Defined Wear Parameter Cards. Additional Card for WEARC.LT.0. Card 3 1 Variable W1 2 W2 3 W3 4 W4 5 W5 6 W6 7 W7 F 0. 8 W8 Type F F F F F F F F Default none none none none none none none none Card 4 is optional. Card 4 1 2 3 4 5 6 7 Variable SFP SFT CID_RCF BT Type F F Default 1.0 1.0 I 0 F 0 8 DT F 1.E20 VARIABLE SLAVE MASTER STYPE MTYPE FricS FricD DAMP DESCRIPTION Node set ID, node ID, part set ID or part ID defining DES on slave side. STYPE below indicates the ID type specified by SLAVE. Part set ID or part ID defining master surface. MTYPE below indicates the ID type specified by MASTER. EQ.0: Slave node set EQ.1: Slave node EQ.2: Slave part set EQ.3: Slave part EQ.0: Part set EQ.1: Part Friction coefficient Rolling friction coefficient Damping coefficient (unitless). If a discrete element sphere impacts a rigid surface with a velocity 𝑣impact, the rebound velocity is 𝑣rebound = (1 − DAMP)𝑣impact BSORT *DEFINE_DE_TO_SURFACE_COUPLING DESCRIPTION Number of cycle between bucket sortings; Default value is 100. For blast simulation with very high DEM particles velocity, it is suggested to set BSORT = 20 or smaller. LT.0: ABS(BSORT) is the minimum number of cycle between bucket sort. This value can be increased during runtime by tracking the velocity of potential coupling pair. This feature only works with MPP currently. LVCx LVCy LVCz Load curve defines surface velocity in 𝑥 direction Load curve defines surface velocity in 𝑦 direction Load curve defines surface velocity in 𝑧 direction WEARC WEARC is the wear coefficient. GT.0: EQ.-1: Archard’s Wear Law, See Remark 1. Finnie Wear Law, additional card is required EQ.-100: User defined wear model, additional card is required W1-W8 WEARC = -1, W1 is yield stress of target material WEARC = -100, user defined wear parameters SFP SFT Scale factor on contact stiffness. By default, SFP = 1.0. The as contact calculated stiffness is 𝐾𝑛 = 𝑆𝐹𝑃 ∙ { 𝐾 ∙ 𝑟 ∙ 𝑁𝑜𝑟𝑚𝐾 𝑖𝑓 𝑁𝑜𝑟𝑚𝐾 > 0 |𝑁𝑜𝑟𝑚𝐾| 𝑖𝑓 𝑁𝑜𝑟𝑚𝐾 < 0 where K is bulk modulus, r is discrete element radius, NormK is scale factor of the spring constant defined in *CONTROL_DISCRETE_ELEMENT. Scale factor for surface thickness (scales true thickness). This option applies only to contact with shell elements. True thickness is the element thickness of the shell elements. CID_RCF Coordinate system ID to output demrcf force resultants in a local system. BT DT Birth time. Death time. Remarks: 1. Archard’s Wear Law. If WEARC > 0 then wear on the shell surface is calculated using Archard’s wear law ℎ̇ = WEARC × 𝑓𝑛 × 𝑣𝑡 where, ℎ = wear depth 𝑓𝑛 = normal contact force from DE 𝑣𝑡 = tangential sliding velocity of the DE on shell 𝐴 = area of contact segment The wear depth is output to the interface force file. 2. Finnie’s Wear Law. If WEARC=-1 then wear on the shell surface is calculated using Finnie’s wear law. The model of Finnie relates the rate of wear to the rate of kinetic energy of particle impact on a surface as: Q = ⎧ 𝑚𝑣2 {{{ 8𝑝 ⎨ 𝑚𝑣2 {{{ 24𝑝 ⎩ (sin 2𝛼 − 3 sin2 𝛼) 𝑖𝑓 tan 𝛼 < cos2 𝛼 𝑖𝑓 tan 𝛼 > where, Q is the volume of the material removed from surface, m is particle mass, α is impact angle and p is the yield stress of the target material, p is read from additional user defined wear parameter card as p = w1.. The wear depth is output to the interface force file. 3. *DATABASE_BINARY_DEMFOR controls the output interval of the coupling forces to the DEM interface force file. This interface force file is activated by the command line option “dem=”, for example, lsdyna i=inputfilename.k … dem=interfaceforce_filename The DEM interface force file can be read into LS-PrePost for plotting of coupling pressure and forces on the master segments. 4. *DATABASE_RCFORC controls the output interval of the coupling forces to the ASCII demrcf file. This output file is analogous to the rcforc file for *CONTACT. *DEFINE_DE_TO_SURFACE_TIED Purpose: To define a tied-with-failure coupling interface between discrete element spheres (DES) and a surface defined by shell part(s) or solid part(s). This coupling is currently not implemented for tshell part(s). Card 1 1 2 3 4 5 6 7 8 Variable SLAVE MASTER STYPE MTYPE Type Default I 0 Card 2 1 I 0 2 I 0 3 I 0 4 5 6 7 8 Variable NFLF SFLF NEN MES LCID NSORT Type F F F Default Required Required 2. F 2. I 0 I 100 VARIABLE SLAVE MASTER STYPE DESCRIPTION Node set ID, node ID, part set ID or part ID defining DES on slave side. STYPE below indicates the ID type specified by SLAVE. Part set ID or part ID defining master surface. MTYPE below indicates the ID type specified by MASTER. EQ.0: Slave node set EQ.1: Slave node EQ.2: Slave part set EQ.3: Slave part MTYPE EQ.0: Part set EQ.1: Part VARIABLE DESCRIPTION NFLF SFLF NEN MES Normal failure force. Only tensile failure, i.e., tensile normal forces, will be considered in the failure criterion Shear failure force Exponent for normal force Exponent for shear force. Failure criterion: ( ∣𝑓𝑛∣ NFLF NEN ) + ( ∣𝑓𝑠∣ SFLF MES ) ≥ 1. Failure is assumed if the left side is larger than 1. 𝑓𝑛 and 𝑓𝑠 are the normal and shear interface force. LCID Load curve ID define the time dependency of failure criterion NSORT Number of cycle between bucket sort Remarks: Both NFLF and SFLF must be defined. If failure in only tension or shear is required then set the other failure force to a large value (1010). *DEFINE_ELEMENT_DEATH_OPTION Available options include: SOLID SOLID_SET BEAM BEAM_SET SHELL SHELL_SET THICK_SHELL THICK_SHELL_SET Purpose: To define a discrete time or box to delete an element or element set during the simulation. This keyword is only for deformable elements, not rigid body elements. Card 1 1 2 3 4 5 6 7 8 Variable EID/SID TIME BOXID INOUT IDGRP CID Type I Default I 0 I 0 I 0 I 0 I 0 VARIABLE DESCRIPTION EID/SID Element ID or element set ID. TIME BOXID Deletion time for elimination of the element or element set. If BOXID is nonzero, a TIME value of zero is reset to 1.0E+16. Element inside or outside of defined box are deleted depending on the value of INOUT. INOUT Location of deleted element: EQ.0: Elements inside box are deleted EQ.1: Element outside of box are deleted VARIABLE IDGRP DESCRIPTION Group ID. All elements sharing the same positive value of IDGRP are considered to be in the same group. All elements in a group will be simultaneously deleted one cycle after any single element in the group fails. There is no requirement that each *DEFINE_ELEMENT_DEATH command have a unique IDGRP. In other words, elements in a single multiple *DEFINE_ELEMENT_DEATH commands. group come from can Elements in which IDGRP = 0 are not assigned to a group and thus deletion of one element does not enforce deletion of the other elements. CID Coordinate ID for transforming box BOXID. If CID is not specified, the box is in the global coordinate system. The box rotates and translates with the coordinate system only if the coordinate system is flagged for an update every time step. *DEFINE_ELEMENT_GENERALIZED_SHELL Purpose: Define a general 3D shell formulation to be used in combination with *ELE- MENT_GENERALIZED_SHELL. The objective of this feature is to allow the rapid prototyping of new shell element formulations by adding them through the keyword input file. All necessary information, like the values of the shape functions and their derivatives at various locations (at the integration points and at the nodal points) have to be defined via this keyword. An example for a 9-noded generalized shell element with 4 integration points in the plane is given in Figure 15-31 to illustrate the procedure. The element formulation ID (called ELFORM) used in this keyword needs to be greater or equal than 1000 and will be referenced through *SECTION_SHELL . Card 1 1 2 3 4 5 6 7 8 Variable ELFORM NIPP NMNP IMASS FORM Type I I I I I Default none none none none none Weights and Shape Function Values/Derivatives at Gauss Points: These cards are read according to the following pseudo code: for i = 1 to NIPP { read cardA1(i) for k = 1 to NMNP { read cardA2(i,k) } } // comment: Read in NIPP × (1 + NMNP) cards Weight Cards. Provide weight for integration point i. (Card A1)i Variable Type 1 2 3 4 5 6 7 8 WI Integration Point Shape Function Value/Derivatives Cards. Provide the value of the kth shape function and its derivative at the ith integration point. (Card A2)ik Variable Type 1 2 3 4 5 6 7 8 NKI F DNKIDR DNKIDS F F For FORM = 0 or FORM = 1, Shape Function Derivatives at Nodes: These cards are read according to the following pseudo code: for l = 1 to NMNP { for k = 1 to NMNP { read cardB(l,k) } } // comment: Read in NMNP × NMNP cards Nodal Shape Function Derivative Cards. The value of the kth shape function’s derivative at the lth nodal point. (Card B)lk 1 2 3 4 5 6 7 8 Variable DNKLDR DNKLDS Type F F For FORM = 2 or FORM = 3, Shape Function 2nd derivative at Gauss Points: NOTE: For FORM = 2 and FORM = 3 it is assumed that the shape functions are at least C1 continuous (having a continuous derivative). The cards for this method are read according to the following pseudo code: for i = 1 to NIPP { for k = 1 to NMNP { read cardB(l,k) } } // comment: Read in NGP × NMNP cards Nodal Shape Function Second Derivative Cards. The value of the kth shape function’s second derivative at the ith integration point. (Card B)ik 1 2 3 4 5 6 7 8 Variable D2NKIDR2 D2NKIDRDS D2NKIDS2 Type F F F VARIABLE ELFORM DESCRIPTION Element Formulation ID referenced via *SECTION_SHELL to connect *ELEMENT_GENERALIZED_SHELL with the appropriate shell formulation. The chosen number needs to be greater or equal than 1000. NIPP Number of in-plane integration points. NMNP Number of nodes for this element formulation. IMASS Option for lumping of mass matrix: EQ.0: row sum EQ.1: diagonal weighting. FORM Shell formulation to be used EQ.0: shear deformable shell theory with rotational DOFs (shell normal evaluated at the nodes) EQ.1: shear deformable shell theory without rotational DOFs (shell normal evaluated at the nodes) EQ.2: thin shell theory without rotational DOFs (shell normal evaluated at the integration points) EQ.3: thin shell theory with rotational DOFs (shell normal evaluated at the integration points) WI Integration weight at integration point i. VARIABLE DESCRIPTION NKI Value of the shape function Nk evaluated at integration point i. DNKIDR Value of the derivative of the shape function Nk with respect to the local coordinate r at the integration point i ( 𝜕𝑁𝑘 𝜕𝑟 ). DNKIDS Value of the derivative of the shape function Nk with respect to the local coordinate s at the integration point i ( 𝜕𝑁𝑘 𝜕𝑠 ). DNKLDR Value of the derivative of the shape function Nk with respect to the local coordinate r at the nodal point l ( 𝜕𝑁𝑘 𝜕𝑟 ). DNKLDS Value of the derivative of the shape function Nk with respect to the local coordinate s at the nodal point l ( 𝜕𝑁𝑘 𝜕𝑠 ). D2NKIDR2 Value of the second derivative of the shape function Nk with respect to the local coordinate r at the integration point i ( 𝜕2𝑁𝑘 𝜕𝑟2 ). D2NKIDRDS Value of the second derivative of the shape function Nk with respect to the local coordinates r and s at the integration point i 𝜕2𝑁𝑘 𝜕𝑟𝜕𝑠 ). ( D2NKIDS2 Value of the second derivative of the shape function Nk with respect to the local coordinate s at the integration point i ( 𝜕2𝑁𝑘 𝜕𝑠2 ). Remarks: 1. For post-processing and the treatment of contact boundary conditions, the use of interpolation shell elements is necessary. 2. The order of how to put in the data for the NMNP nodal points has to be in correlation with the definition of the connectivity of the element in *ELE- MENT_GENERALIZED_SHELL. *DEFINE_ELEMENT_GENERALIZED_SHELL II III IV Connectivity of Generalized-Shell Element Generalized-Shell Element Integration Point *DEFINE_ELEMENT_GENERALIZED_SHELL $# elform 1001 nmnp 9 nipp 4 $# integration point 1 (i=1) $# wi 1.3778659577546E-04 imass 0 form $# dnkids 1.7098997698601E-01 3.3723996630918E+00 2.4666694616947E+00 dnkidr nki ... $# integration point 2 (i=2) 2.2045855324077E-04 5.4296436772101E-02 1.9003752917745E+00 7.8327025592051E+00 Block A ... $# integration point 3 (i=3) ... $# integration point 4 (i=4) ... $# node 1 (l=1) $# dnkldr dnklds 4.8275862102259E+00 3.5310344763662E+01 ... $# node 2 (l=2) 2.4137931051130E+00 8.8275861909156E+00 Block B ... [...] $# node 9 (l=9) ... W1 k=1 k=2-9 W2 NMNP Lines 1 (W3)+ NMNP Lines 1 (W4)+ NMNP Lines k=1 k=2-9 NMNP Lines NMNP Lines Figure 15-31. Example of a generalized shell formulation with *DEFINE_ELE- MENT_GENERALIZED SHELL. *DEFINE_ELEMENT_GENERALIZED_SOLID Purpose: Define a general 3D solid formulation to be used in combination with *ELE- MENT_GENERALIZED_SOLID. The objective of this feature is to allow the rapid prototyping of new solid element formulations by adding them through the keyword input file. All necessary information, like the values of the shape functions and their derivatives at all integration points have to be defined via this keyword. An example for a 18-noded generalized solid element with 8 integration points is given in Figure 15-31 to illustrate the procedure. The element formulation ID (called ELFORM) used in this keyword needs to be greater or equal than 1000 and will be referenced through *SECTION_SOL- ID . Card 1 1 2 3 4 5 6 7 8 Variable ELFORM NIP NMNP IMASS Type I I I I Default none none none none These cards are read according to the following pseudo code: for i = 1 to NIP { read cardA1(i) for k = 1 to NMNP { read cardA2(i,k) } } // comment: Read in NIP × (1 + NMNP) cards Weight Cards. Provide weight for integration point i. (Card A1)i Variable Type 1 2 3 4 5 6 7 8 WI F Default none Integration Point Shape Function Value/Derivatives Cards. Provide the value of the kth shape function and its derivative at the ith integration point. (Card A2)ik Variable Type 1 2 3 4 5 6 7 8 NKI F DNKIDR DNKIDS DNKIDT F F F Default none none none none VARIABLE ELFORM DESCRIPTION Element Formulation ID referenced via *SECTION_SOLID to connect *ELEMENT_GENERALIZED_SOLID with the appropriate solid formulation. The chosen number needs to be greater or equal than 1000. NIP Number of integration points. NMNP Number of nodes for this element formulation. IMASS Option for lumping of mass matrix: EQ.0: row sum EQ.1: diagonal weighting. Integration weight at integration point i. Value of the shape function Nk evaluated at integration point i. WI NKI DNKIDR Value of the derivative of the shape function Nk with respect to the local coordinate r at the integration point i ( 𝜕𝑁𝑘 𝜕𝑟 ). DNKIDS Value of the derivative of the shape function Nk with respect to the local coordinate s at the integration point i ( 𝜕𝑁𝑘 𝜕𝑠 ). DNKIDT Value of the derivative of the shape function Nk with respect to the local coordinate t at the integration point i ( 𝜕𝑁𝑘 𝜕𝑡 ). Remarks: 1. For post-processing the use of interpolation solid elements is necessary. 2. The order of how to put in the data for the NMNP nodal points has to be in correlation with the definition of the connectivity of the element in *ELEMENT_ GENERALIZED_SOLID. Example: VI 11 II 12 10 13 VII 14 VIII III 16 15 17 IV 18 *DEFINE_ELEMENT_GENERALIZED_SOLID $# elform 1001 nmnp 18 nip 8 $# integration point 1 (i=1) $# wi 1.3778659577546E-04 Connectivity of Generalized-Solid Element Generalized-Solid Element Integration Point imass W1 k=1 k=2,18 W2 NMNP Lines W8 NMNP Lines $# dnkidt 1.7098997698601E-01 3.3723996630918E+00 2.4666694616947E+00 1.5327451653258E+00 dnkidr dnkids nki ... $# integration point 2 (i=2) 2.2045855324077E-04 5.4296436772101E-02 1.9003752917745E+00 7.8327025592051E+00 3.258715871621E+00 ... [...] $# integration point 8 (i=8) Block A 3.8574962585875E-04 2.6578426581235E-01 1.6258741125438E+00 2.9876495873627E+00 5.403982758392E+00 ... Figure 15-32. Example of a generalized solid formulation with *DEFINE_EL- EMENT_GENERALIZED_SOLID *DEFINE_FABRIC_ASSEMBLIES Purpose: Define lists of part sets to properly treat fabric bending between parts. Define as many cards as needed for the assemblies, using at most 8 part sets per card. This input ends at the next keyword (“*”) card. Card 1 1 2 3 4 5 6 7 8 Variable SPID1 SPID2 SPID3 SPID4 SPID5 SPID6 SPID7 SPID8 Type Default I 0 I 0 I 0 I 0 I 0 I 0 I 0 I 0 VARIABLE DESCRIPTION SPIDn Part set ID that comprises an assembly. Remarks: The materials *MAT_FABRIC and *MAT_FABRIC_MAP are equipped with an optional coating feature to model the fabric’s bending resistance. See the related parameters ECOAT, SCOAT and TCOAT on these material model manual entries. The default behavior for these coatings, which this keyword changes, excludes T- interesections, and, furthermore requires that all fabric elements must have a consistently oriented normal vector. In Figure 15-33, the left connection of fabric elements is permitted by the default functionality while the right one is not. However, with using this keyword the proper bending treatment for the right connectivity can be activated by adding the following input to the deck 1 2 15-33. Figure Bending *DEFINE_FABRIC_ASSEMBLIES. elements belong to. in fabric, The numbers intended of indicate the parts the use *SET_PART_LIST 1 1,2 *SET_PART_LIST 2 3 *DEFINE_FABRIC_ASSEMBLIES 1,2 which decouples part 3 from the other two parts in terms of bending, thus creating a moment free hinge along the edge between part sets 1 and 2. Bending between parts 1 and 2 is unaffected since these are contained in the same fabric assembly. For several instances of this keyword in an input deck, the list of assemblies is appended. If assemblies are defined and there happens to be fabric parts that do not belong to any of the specified assemblies, then these parts are collected in a separate unlisted assembly. The restriction on consistent normal vectors and on having no T- intersections applies to all elements within an assembly. *DEFINE_FILTER Purpose: Define a general purpose filter, currently used by this option: SENSOR_SWITCH The input in this section consists of two cards: Card 1 Variable 1 ID Type I 2 3 4 5 6 7 8 Title A70 Card 2 1 2 3 4 5 6 7 8 Type Type Data1 Data2 Data3 Data4 Data5 Data6 Data7 Type A10 VARIABLE DESCRIPTION ID Title Type Identification number. Title for this filter. One of CONTINUOUS, or CHAIN the 3 currently defined filter types: DISCRETE, Data1-7 Filter type specific data, which determines what the filter does. Filter Types: FILTER DISCRETE DESCRIPTION The discrete filter operates on a fixed number of values of the input data. The first data field is an A10 character field, which gives the type of operation the filter performs: MIN, MAX, and AVG are the available options. The second data field is an I10 field, giving the number of input values over which the minimum, maximum, or average is computed. CONTINUOUS CHAIN *DEFINE DESCRIPTION Similar to the DISCRETE filter, except that it operates over a fixed time interval. The first data field is exactly the same as for the DISCRETE option. The second data field is an F10 field, indicating the duration of the filter. For example, if AVG is given, and the duration is set to 0.1, a running timestep weighted average is computed over the last 0.1 time of the simulation. Here, data fields 1-7 are all I10 fields, and give the IDs of a list of other filters (including other CHAIN filters, if desired), each of which will be applied in order. So the raw data is fed to the filter indicated by Data1. The output of that is fed to the next filter, and so on, with up to 7 filters in the chain. List only as many filters as you need. *DEFINE_FORMING_BLANKMESH Purpose: This keyword, together with keyword *ELEMENT_BLANKING, enable mesh generation for a sheet metal blank. This keyword is renamed from the previous keyword *CONTROL_FORMING_BLANKMESH. The keyword *DEFINE_CURVE_- TRIM_NEW can be coupled with this keyword to define a blank with a complex periphery and a number of inner hole cutouts. Card 1 1 2 3 4 5 6 7 8 Variable IDMSH ELENG XLENG YLENG ANGLEX NPLANE CID Type I F F F F Default none 0.0 0.0 0.0 0.0 Card 2 1 2 3 4 5 I 1 6 I 0 7 8 Variable PIDBK NID EID XCENT YCENT ZCENT XSHIFT YSHIFT Type Default I 1 I 1 I 1 F F F F F 0.0 0.0 0.0 0.0 0.0 VARIABLE DESCRIPTION IDMSH ID of the blankmesh (not the blank PID); must be unique. ELENG Element edge length. XLENG YLENG ANGLEX Length of the rectangular blank along X-axis in the coordinate system (CID) defined. Length of the rectangular blank along Y-axis in the coordinate system (CID) defined. An angle defined about Z-axis of the CID specified, starting from the X-axis as the zero degree, to rotate the blank and the orientation of the mesh to be generated. The sign of the rotation angle follows the right hand rule. See Remark 3. VARIABLE NPLANE DESCRIPTION Plane in which a flat blank to be generated, in reference to the coordinate system defined (CID): EQ.0 or 1: XY-plane (default) EQ.2: EQ.3: XZ-plane YZ-plane CID ID of the local coordinate system, defined by *DEFINE_COORDI- NATE_SYSTEM. Default is 0 representing global coordinate system. PIDBK Part ID of the blank, as defined by *PART. NID EID Starting node ID of the blank to be generated. Starting element ID of the blank to be generated. XCENT X-coordinate of the center of the blank. YCENT Y-coordinate of the center of the blank. ZCENT Z-coordinate of the center of the blank. XSHIFT YSHIFT Blank shifting distance in X-axis in coordinate system defined (CID). Blank shifting distance in Y-axis in coordinate system defined (CID). About the keyword: A rectangular blank is defined and meshed, which can be trimmed with IGES curves to a desired periphery and inner cutouts. This keyword is used in conjunction with keyword *ELEMENT_BLANKING. The blank outlines and inner holes can be defined using keyword *DEFINE_CURVE_TRIM_NEW. Application example: A partial keyword example of generating a flat blank with PID 1 is provided blow. Referring to Figure 15-34, the blank mesh is to be generated in XY plane in a global coordinate system, with an average element edge length of 12 mm and a blank dimension of 1100.0 x 1050.0 mm, with node and element ID starting at 8000, and with the center of the blank in the global origin. The blank is to be trimmed out with an inner cut-out hole, given by the IGES file innerholes.iges. Blank outer line is defined with an IGES file outerlines.iges. Both IGES files are used to trim the rectangular blank using keyword *DEFINE_CURVE_TRIM_NEW, where the variable TFLG is used to indicate whether it is an inside or outside trim. The blank generated for example is shown in Figure 15-35. *KEYWORD $---+----1----+----2----+----3----+----4----+----5----+----6----+----7----+----8 *CONTROL_TERMINATION $# endtim 0.000 *CONTROL_FORMING_BLANKMESH $ IDMSH ELENG XLENG YLENG ANGLEX NPLANE CID 3 12.00 1100.00 895.0 0.0 0 0 $ PIDBK NID EID XCENT YCENT ZCENT XSHIFT YSHIFT 1 8000 8000 *ELEMENT_BLANKING $# psid 1 *DEFINE_CURVE_TRIM_NEW $# tcid tctype TFLG TDIR TCTOL TOLN NSEED1 NSEED2 11111 2 1 0 0.250000 1.000000 innerholes.iges *DEFINE_CURVE_TRIM_NEW $# tcid tctype TFLG TDIR TCTOL TOLN NSEED1 NSEED2 11112 2 -1 0 0.250000 1.000000 outerlines.iges *CONTROL_SHELL ...... *CONTROL_SOLUTION ...... *DATABASE_BINARY_D3PLOT ...... *DATABASE_EXTENT_BINARY ...... *SET_PART_list 1 1 *PART Blank $# pid secid mid 1 1 1 *SECTION_SHELL $# secid elform shrf nip propt qr/irid icomp setyp 1 16 0.833000 7 1 0 0 0 $# t1 t2 t3 t4 nloc marea idof edgset 1.500000 1.500000 1.500000 1.500000 0.000 0.000 0.000 0 *MAT_037 $# mid ro e pr sigy etan r hlcid 1 7.9000E-9 2.0700E+5 0.300000 253.25900 0.000 1.408000 90903 *DEFINE_CURVE 90903 253.2590027 ...... 0.9898300 616.7999878 *INTERFACE_SPRINGBACK_LSDYNA $# psid nshv 1 1000 *END The blank and mesh orientation can be rotated about Z-axis defined. Following the right hand rule, the blank in this case is rotated about Z-axis for a positive 30°, as shown in Figure 15-35, with the angle of 0° aligned with X-axis. Inner hole and outer periphery can also be trimmed using the NSEEDs variables in keyword *DEFINE_CURVE_TRIM_NEW. Revision information: This feature is available in LS-DYNA Revision 59165 or later releases. The keyword name change from *CONTROL… to *DEFINE… started in Revision 69074. The variable NPLANE is implemented in Revision 69128 and later releases. Blank outlines (outlines.iges) Inner cutout (innerhole.iges) Regutangular blank of 1100.0x1050.0mm Figure 15-34. Initial input for a blank meshing. 30 deg. Figure 15-35. Resulting blank mesh. *DEFINE_FORMING_CLAMP Purpose: This keyword simplifies the process definition during a clamping simulation, and works as a macro serving as a placeholder for the combination of cards needed to model a clamping process such as those that are commonly used in sheet metal forming. A related keyword includes *DEFINE_FORMING_CONTACT. Define Clamp Card. Define one card for each clamp set. Include as many cards in the following format as desired. This input ends at the next keyword (“*”) card. Card 1 1 2 3 4 Variable CLP1 CLP2 VID GAP Type I I I F 5 AT F 6 DT F 7 8 Default none none none 0.0 0.0 0.0 VARIABLE DESCRIPTION CLP1 CLP2 Part ID of a moving rigid body clamp, defined by *PART and *MAT_020 (*MAT_RIGID). Part ID of a fixed rigid body clamp, defined by *PART and *MAT_020. This is sometimes called “net pad”. VID Define CLP1 moving direction: GT.0: Vector ID from *DEFINE_VECTOR, specifying the moving direction of CLP1 LT.0: Absolute value is a node ID, whose normal vector will be used to define the moving direction of CLP1. Final desired distance between CLP1 and CLP2 at the end of clamping. Begin time for CLP1’s move. Duration of CLP1’s move. GAP AT DT *DEFINE One typical application of this keyword is to estimate springback during the clamping of a formed panel on a checking fixture. Net pads (lower fixed regular or square pads) of a few millimeters thick are placed according to GD&T (Geometry Dimensioning and Tolerancing) requirements on a support platform, typically taking shape of the nominal product. Each net pad (CLP2, see Figure 15-36) has a corresponding moving clamp (CLP1). The movable clamp (CLP1) is initially open so that the formed panel can be loaded onto the net pads. Four-way and two-way position gaging pins are used to initially locate and load the panel in the fixture, before CLP1 is moved to close with the net pad (CLP2). A white light scan is then performed on the panel and scan data is processed to ascertain the degree of panel conformance to the required nominal shape. Even with the clamps fully closed, some severely distorted panels will significantly deviate from the nominal shape when the residual stresses from the forming process are too great. Although, unrelated to this keyword another common method to determine the panel springback amount is the free state check which involves a white light scan on the panel secured on a platform but with no additional forces (clamps – CLP1s) applied to deform the panel (to the net pads CLP2s, for example). LS-DYNA can model both methods and job setups can be easily done by selecting Implicit Static Flanging process in LS-PrePost 4.2’s eZ-Setup (http://ftp.lstc.com/anonymous/outgoing/lsprepost/4.2/win64/). Furthermore, once springback has been determined die compensation (*INTERFACE_COMPENSATION_- NEW) can then be performed to minimize or eliminate the springback; the resulting compensated die shapes can be surfaced, re-machined to produce panels that are within dimensional tolerance. Application Forming Metal / Since the clamp is, typically, modelled with a much coarser mesh than that on a blank, *CONTACT_FORMING_SURFACE_TO_SURFACE should be used. Rotating-type of clamps are currently not supported. Application example: A partial keyword example of using the feature is listed below. Referring to Figure 15-36, the drawn and trimmed blank is positioned between the clamps CLP1 and CLP2. The implicit termination “time” is set at 1.0, with a stepping size of 0.25, for a total of four steps – two steps each for the two CLP1. With the original blank thickness of 1.0 mm, the CLP1s are set to close with the lower CLP2s at “time” of 1.0, leaving a total GAP of 1.02 mm. Note the VIDs are defined as “-46980”, indicating that the moving clamps (CLP1) will move in the normal direction defined by Node #46980. The contact definition using between *DEFINE_FORMING_CONTACT. defined clamps panel and the the are *KEYWORD *INCLUDE ./trimmed.dynain ./nets.k *CONTROL_TERMINATION 1.0 *CONTROL_IMPLICIT_forming 1 *control_implicit_general 1,0.25 *CONTROL_SHELL ⋮ *DATABASE_EXTEND_BINARY ⋮ *PART Blank $ PID SECID MID 1 1 1 Clamp1 2,2,2 Clamp2 3,2,3 Clamp3 4,2,2 Clamp4 5,2,3 *MAT_TRANSVERSELY_ANISOTROPIC_ELASTIC_PLASTIC $ MID RO E PR SIGY ETAN R HLCID 1 2.700E-09 12.00E+04 0.28 0.0 0.0 0.672 2 *MAT_RIGID $# mid ro e pr n couple m alias 2 7.8500E-9 2.1000E+5 0.300000 $# cmo con1 con2 1.000000 7 7 $# lco or a1 a2 a3 v1 v2 v3 0.000 0.000 0.000 0.000 0.000 0.000 *MAT_RIGID $# mid ro e pr n couple m alias 3 7.8500E-9 2.1000E+5 0.300000 $# cmo con1 con2 1.000000 4 7 $# lco or a1 a2 a3 v1 v2 v3 *SETION_SHELL 1,16,,7 1.0,1.0,1.0,1.0 *LOAD_BODY_Z 9997 1.0 *DEFINE_CURVE 9997 0.0000 9810.0000 1.0000 9810.0000 *DEFINE_FORMING_CLAMP $---+----1----+----2----+----3----+----4----+----5----+----6----+----7----+----8 $ CLP1 CLP2 VID GAP AT DT 3 2 -46980 1.02 0.0 0.5 5 4 -46980 1.02 0.5 0.5 $---+----1----+----2----+----3----+----4----+----5----+----6----+----7----+----8 *DEFINE_FORMING_CONTACT $ IPS IPM FS ONEWAY 1 2 0.125 1 1 3 0.125 1 1 4 0.125 1 1 5 0.125 1 *END Note with this keyword, formed panel needs to be pre-positioned properly with respect to the clamps by users, and auto-position (*CONTROL_FORMING_AUTOPOSITION) cannot be used. Furthermore, prescribed motions and clamp motion curves do not need to be defined for the clamps. Revision information: This feature is available starting in double precision LS-DYNA Revision 99007 for implicit static only. Element normals of the moving clamps Element normals of the net pads Initial position (side view); t=0.0 First clamp moving down half- way; panel springs back; t=0.25 First clamp completes moving; t=0.50 GAP Second clamp moving down half-way; t=0.75 Second clamp completes moving (fully clamped); t=1.0 Formed & trimmed blank (before springback) Fixed net pads (CLP2) Node 46980 Second moving clamp (CLP1) First moving clamp (CLP1) Initial position (iso-view); t=0.0 Fully clamped position (iso-view) t=1.0 Figure 15-36. Variable definitions and an example of using the negative VID. *DEFINE Purpose: This keyword works as macro for the FORMING_(ONE_WAY)_SURFACE_- TO_SURFACE keyword. It adds one contact definition to the model per data card. Each data card consists of a reduced set of FIELDS compared with the full *CONTACT keyword. The omitted fields take their default values. A related keyword includes *DEFINE_FORMING_CLAMP. Define Contact Card. Define one card for each contact interface. Define as many cards in the following format as desired. The input ends at the next keyword (“*”) card. Card 1 1 2 3 4 5 6 7 8 Variable IPS IPM FS ONEWAY Type I I F Default none none none I 0 VARIABLE DESCRIPTION IPS IPM Part ID of a slave sliding member, typically a deformable sheet metal blank. Part ID of a master sliding member, typically a tool or die defined as a rigid body. Deformable blank PID 1 Fixed net pad PID 5 Clamp PID 2 Fixed net pad PID 4 Clamp PID 3 Figure 15-37. Define contact interfaces. *DEFINE_FORMING_CONTACT DESCRIPTION FS Coulomb friction coefficient. ONEWAY Define FORMING contact type: EQ.0: The contact is FORMING_ONE_WAY_SURFACE_TO_- SURFACE. EQ.1: The contact is FORMING_SURFACE_TO_SURFACE. Application example: A partial keyword example of defining contact between a deformable part and two pairs of clamps is given below. In Figure 15-37, a blank PID of 1 is defined to have FORMING_SURFACE_TO_SURFACE contact with rigid body clamps of PID of 2, 3, 4, and 5, with coefficient of frictions for each interface as 0.125, 0.100, 0.125, and 0.100, respectively. Only a total of four lines are needed to define four contact interfaces, as opposed to at least three cards for each interface. $---+----1----+----2----+----3----+----4----+----5----+----6----+----7----+----8 *DEFINE_FORMING_CONTACT $ IPS IPM FS ONEWAY 1 2 0.125 1 1 3 0.100 1 1 4 0.125 1 1 5 0.100 1 Revision information: This feature is available starting in LS-DYNA Revision 98988. *DEFINE Purpose: Define friction coefficients between parts for use in the contact options: SINGLE_SURFACE, AIRBAG_SINGLE_SURFACE, AUTOMATIC_GENERAL, AUTOMATIC_SINGLE_SURFACE, AUTOMATIC_SINGLE_SURFACE_MORTAR, AUTOMATIC_NODES_TO_SURFACE, AUTOMATIC_SURFACE_TO_SURFACE, AUTOMATIC_SURFACE_TO_SURFACE_MORTAR, AUTOMATIC_ONE_WAY_SURFACE_TO_SURFACE, ERODING_SINGLE_SURFACE. The input in this section continues until then next “*” card is encountered. Default friction values are used for any part ID pair that is not defined. The coefficient tables specified by the following cards are activated when FS is set to -2.0. This feature overrides the coefficients defined in *PART_CONTACT (which are turned on only when FS is set to -1.0). When only one friction table is defined, it is used for all contacts having FS set to -2. Otherwise, for each contact with FS equal to -2, the keyword reader assigns a table to each *CONTACT by matching the value of FD from *CONTACT with an ID from Card 1 below. Failure to match FD to an ID causes error termination. Card 1 Variable Type Default 1 ID I 0 2 3 4 5 6 7 8 FS_D FD_D DC_D VC_D F F F F 0.0 0.0 0.0 0.0 Friction ij card. Sets the friction coefficients between parts i and j. Add as many of these cards to the deck as necessary. The next keyword (“*”) card terminates the friction definition. Card 2… 1 Variable PIDi 2 PIDj 3 FSij 4 FDij 5 DCij 6 7 8 VCij PTYPEi PTYPEj Type I I F F F F A A Default 0.0 0.0 0.0 0.0 VARIABLE DESCRIPTION ID FS_D FD_D DC_D Identification number. Only one table is allowed. Default value of the static coefficient of friction. The frictional coefficient is assumed to dependend on the relative velocity 𝑣rel of the surfaces in contact, 𝜇𝑐 = FD + (FS − FD)𝑒−DC∣𝑣rel∣. Default values are used when part pair are undefined. For mortar contact 𝜇𝑐 = FS, i.e., dynamic effects are ignored. Default value of the dynamic coefficient of friction. The frictional coefficient is assumed to depended on the relative velocity 𝑣rel of the surfaces in contact, 𝜇𝑐 = FD + (FS − FD)𝑒−DC∣𝑣re𝑙∣. Default values are used when part pair are undefined. For mortar contact 𝜇𝑐 = FS, i.e., dynamic effects are ignored. Default value of the exponential decay coefficient. The frictional coefficient is assumed to be depend on the relative velocity 𝑣rel of the surfaces in contact, 𝜇𝑐 = FD + (FS − FD)𝑒−DC∣𝑣rel∣. Default values are used when part pair are undefined. For mortar contact 𝜇𝑐 = FS, i.e., dynamic effects are ignored. VARIABLE VC_D DESCRIPTION Default value of the coefficient for viscous friction. This is necessary to limit the friction force to a maximum. A limiting force is computed 𝐹lim = VC × 𝐴cont, where 𝐴cont is the area of the segment contacted by the node in contact. The suggested value for VC is to use the yield stress in where σo is the yield stress of the contacted shear VC = 𝜎𝑜 √3 material. Default values are used when part pair are undefined. PIDi PIDj FSij FDij DCij VCij PTYPEi, PTYPEj Part, or part set, ID i. Part, or part set, ID j. Static coefficient of friction between parts i and j. Dynamic coefficient of friction between parts i and j. Exponential decay coefficient between parts i and j. Viscous friction between parts i and j. EQ.“PSET”: when PTYPEi or PTYPEj refers to a *SET_PART. *DEFINE_FRICTION_ORIENTATION Purpose: This keyword allows for definition of different coefficients of friction (COF) in specific directions, specified using a vector and angles in degree. In addition, COF can be scaled according to the amount of pressure generated in the contact interface. This feature is intended for use with FORMING_ONE_WAY type of contacts. This feature is developed jointly with the Ford Motor Company. Card 1 1 2 3 Variable PID LCID LCIDP Type I Default none I 0 I 0 7 8 4 V1 F 5 V2 F 6 V3 F 0.0 0.0 0.0 DESCRIPTION VARIABLE PID Part ID to which directional and pressure-sensitive COF is to be applied. See *PART. LCID ID of the load curve defining COF vs. orientation in degree. LCIDP ID of the load curve defining COF scale factor vs. pressure. V1 V2 V3 Vector components of vector V defining zero-degree (rolling) direction. Vector components of vector V defining zero-degree (rolling) direction. Vector components of vector V defining zero-degree (rolling) direction. The assumption: Load curves LCID and LCIDP are not extrapolated beyond what are defined. It is recommended that the definition is specified for the complete range of angle and pressure expected. One edge of all elements on the sheet metal blank must align initially with the vector defined by V1, V2, and V3. Application example: The following is a partial keyword input of using this feature to define directional frictions and pressure-sensitive COF scale factor. *DEFINE_FRICTION_ORIENTATION $ PID LCID LCIDP V1 V2 V3 1 15 16 1.0 0. 0. $$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ $ define COF vs. orientation angle *DEFINE_CURVE 15 0.0, 0.3 90.0, 0.0 $$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ $ define COF scale factor vs. pressure *DEFINE_CURVE 16 0.1, 0.3 0.2, 0.3 0.3, 0.3 0.4, 0.2 0.5, 0.5 0.6, 0.4 Referring to Figure 15-38, a deformable blank is clamped with 1000N of force between two rigid plates and is pulled along the direction of X-axis for 90 mm using displacement control. Initial and final positions of the blank are shown in Figure 15-39. The normal force is recovered from RCFORC file, as shown in Figure 15-40, which agrees with what is applied. Frictional force (pulling force) in X-direction is plotted as 89N, shown in Figure 15-41. A hand calculation from the input verifies this result: [clamping force] ⏟⏟⏟⏟⏟⏟⏟⏟⏟ 1000𝑁 × [𝑥-dir coefficient] ⏟⏟⏟⏟⏟⏟⏟⏟⏟ 0.3 × [coefficient scale factor at 0.27 pressure] ⏟⏟⏟⏟⏟⏟⏟⏟⏟⏟⏟⏟⏟⏟⏟⏟⏟⏟⏟⏟⏟ 0.3 = 90𝑁 The interface pressure can be output from an LS-DYNA run when ‘S = filename’ is included in the command line. The binary output can be viewed from LS-PrePost4.0. The element directions are automatically aligned with the vector V. The left side of Figure 15-42 shows the element directions of the incoming sheet blank. The keyword will re-orient the element directions based on the vector V specified, which has the component of [1.0, 0.0, 0.0] in this case. The re-oriented element directions for the blank are shown on the right side of the Figure. Following the numeric directions provided in Figure 15-43, LS-PrePost4.0 can be used to check the element directions of a sheet blank. This feature is generally developed for use with FORMING_ONE_WAY type of contact in SMP. However, this keyword can be used in combination with *CONTACT_FORM- ING_ONE_WAY_SURFACE TO_SURFACE_ORTHO_FRICTION, and in fact, it can only be used in this manner if running MPP. In this combination, the variables LCID and LCIDP are overridden by friction factor input in ORTHO_FRICTION, while the vector [V1, V2, V3] defines the first orthogonal direction. It furthermore allows the convenience of SSID and MSID in *CONTACT being input as part set IDs (when SSTYP/MSTYP = 2), in which case the segments sets necessary for ORTHO_FRICTION are generated automatically with orientation according to the vectors defined by [V1, V2, V3]. The part set ID input option is typically used by metal forming users. A detailed keyword example is shown in Figure 15-44. Revision information: This feature is available in LS-DYNA Revision 60275 and later releases for SMP. It works with MPP with one way forming type of contact with ORTHO_FRICTION starting from Rev 73226. In addition, it works with SMOOTH contact option starting from Revision 69631. 1000N applied on upper rigid plate, about 0.27 N/mm2 of pressure on the deformable blank. Lower rigid plate fixed, of size 169 x 169mm Pull 90mm in X on each node along the edge of a deformable blank of size 61.25 x 61.25mm) Figure [15-38]. Boundary and loading conditions of a small test model. max=90.0045, at node #149 X-displacement (mm) Final position Initial position 90 81 72 63 54 45 36 27 18 Figure [15-39]. Initial and final position of the blank. -0.2 -0.4 -0.5 -1 ) ( - -1.2 0.05 0.1 0.15 Time (sec) Figure [15-40]. Normal force from RCFORC file. ) ( - 100 80 60 40 20 0.05 0.1 0.15 Time (sec) Figure [15-41]. Pulling force (frictional force) from RCFORC file. Figure [15-42]. Element directions (N1-N2) of an incoming sheet blank (left) and directions after re-orientation. Identify Element Particle Node Part CNRB Shell Solid Beam Seat. SPH Mass Disc. DiscSph. Iner. Nurbs Tshel AnyE Key in xyz coord Show Results Elem Dir Mat Dir No ID AirbagR Show Popup Echo Ident RefGeo Find Curve Blank Surf MovCop Solid Offset GeoTol Transf Mesh Normal Model DetEle EleTol DupNod Post NodEdit MFPre Part Name EleEdit MFPost Measur Favor1 Clear Node Clear Elem Clear All Clear Node Clear Elem Clear All Clear Node Clear Elem Clear All ByNode ByElem ByPart ByGpart BySubsys BySET ByEdge ByPath BySegm ByCurve BySurf Total identified nodes: Total identified elems: Total identified parts: Total identified particles: Total identified CNRBs: Clear Node Clear Part Clear Elem Clear CNRB Clear All Done Sel. Elem. (0) Pick Area Poly Sel1 Sphe Box Prox Circ Frin Plan In Out Add Rm ID Type any Label selection 3DSurf Figure [15-43]. Checking element directions (N1-N2) by part using LS- PrePost4.0. *DEFINE_FRICTION_ORIENTATION $ PID LCID LCIDP V1 V2 V3 1,,, 1.0 0.0 0.0 *CONTACT_FORMING_ONE_WAY_SURFACE_TO_SURFACE_ORTHO_FRICTION $ SSID MSID SSTYP MSTYP 1, 3, 2, 2 $ FS FD DC VC 1.25, 0.0, 20.0 $ SFS SFM 0.0, 0.0 $FS1_S, FD1_S, DC1_S, VC1_S, LC1_S, OACS_S, LCFS, LCPS 0.3, 0.0, 0.0, 0.0,, , 1, 15, 16 $FS2_S, FD2_S, DC2_S, VC2_S, LC2_S 0.1, 0.0, 0.0, 0.0 $FS1_M, FD1_M DC1_M, VC1_M, LC1_M, OACS_M, LCMS, LCPM 0.3, 0.0, 0.0, 0.0, , 0, 15, 16 $FS2_M, FD2_M, DC2_M, VC2_M, LC2_M 0.1, 0.0, 0.0, 0.0 *DEFINE_CURVE $ LCFS, define COF vs. angle based on 1st orthogonal direction 15 0.00,0.3 45.0,0.2 90.0,0.1 *DEFINE_CURVE $ LCPS, define COF scale factor vs. pressure 16 0.0,0.0 0.3,0.3 0.5,0.5 Use this keyword/vector to define rolling direction Use *Set_part_list FS ignored if ORTHO_FRICTION is present FS1_S, LC1_S ignored if LCFS, LCPS are defined: LCFS: COF vs. Angle; LCPS: COF scale factor vs. Pressure. FS1_M, LC1_M ignored if LCFM, LCPM are defined 1st Orthogonal direction follows slave segment orientation, as defined by ‘a1’ in *SET_SEGMENT; Ignored when defined with *DEFINE_FRICTION_ORIENTATION. 1st Orthogonal direction follows slave segment orientation, as defined by ‘a1’ in *SET_SEGMENT; Ignored when defined with *DEFINE_FRICTION_ORIENTATION. Figure [15-44]. Use of this keyword with _ORTHO_FRICTION for MPP. *DEFINE Purpose: Define a function that can be referenced by a limited number of keyword options. The function arguments are different for each keyword that references *DE- FINE_FUNCTION. Unless stated otherwise, all the listed argument(s) in their correct order must be included in the argument list. Some usages of *DEFINE_FUNCTION allow random ordering of arguments and argument dropouts. See the individual keywords for the correct format. Some examples are shown below. The TITLE option is not allowed with *DEFINE_FUNCTION. Card 1 1 2 3 4 5 6 7 8 Variable FID Type I HEADING A70 Function Cards. Insert as many cards as needed. These cards are combined to form a single line of input. The next keyword (“*”) card terminates this input. Card 1 2 3 4 5 6 7 8 Variable Type VARIABLE FID FUNCTION A80 DESCRIPTION Function ID. Functions, tables , and load curves may not share common ID's. A unique number has to be defined. HEADING An optional descriptive heading. FUNCTION Arithmetic expression involving a combination of independent variables and other functions, i.e., “f(a,b,c)=a*2+b*c+sqrt(a*c)” where a, b, and c are the independent variables. The function name, “f(a,b,c)”, must be unique since other functions can then use example, “g(a,b,c,d)=f(a,b,c)**2+d”. In this example, two *DEFINE_FUNC- TION definitions are needed to define functions f and g. reference function. and this For *DEFINE_FUNCTION The following examples serve only as an illustration of syntax. Unlike *DEFINE_CURVE and *DEFINE_CURVE_FUNCTION, *DEFINE_FUNCTION is always active in dynamic relaxation phase. Example 1: Prescribe sinusoidal 𝑥-velocity and 𝑧-velocity for some nodes. *BOUNDARY_PRESCRIBED_MOTION_SET $# nsid dof vad lcid sf 1 1 0 1 1 3 0 2 *DEFINE_FUNCTION 1,x-velo x(t)=1000*sin(100*t) *DEFINE_FUNCTION 2,z-velo a(t)=x(t)+200 Example 2: Ramp up a hydrostatic pressure on a submerged surface. *comment units: mks Apply a hydrostatic pressure ramped up over a finite time = trise. pressure on segment = rho * grav * depth of water where depth of water is refy - y-coordinate of segment and refy is the y-coordinate of the water surface *DEFINE_FUNCTION 10 float hpres(float t, float x, float y, float z, float x0, float y0, float z0) { float fac, trise, refy, rho, grav; trise = 0.1; refy = 0.5; rho = 1000.; grav = 9.81; fac = 1.0; if(t<=trise) fac = t/trise; return fac*rho*grav*(refy-y); } *LOAD_SEGMENT_SET 1,10 Example 2 illustrates that a programming language resembling C can be used in defining a function. Before a variable or function is used, its type must be declared; that is the purpose of "float" (i.e., a real variable rather than integer type) appearing before those entities. The braces indicate the beginning and end of the function being programmed. Semicolons must appear after each statement but several statements may appear on a single line. Please refer to a C programming guide for more detailed information. *DEFINE_FUNCTION_TABULATED Purpose: Define a function of one variable using two columns of input data (in the manner of *DEFINE_CURVE) that can be referenced by a limited number of keyword options or by other functions defined via *DEFINE_FUNCTION. The TITLE option is not allowed with *DEFINE_FUNCTION_TABULATED. Card 1 1 2 3 4 5 6 7 8 Variable FID Type I HEADING A70 Card 2 1 2 3 4 5 6 7 8 Variable Type FUNCTION A80 Point Cards. Put one pair of points per card (2E20.0). Add as many cards as necessary. Input is terminated when a keyword (“*”) card is found. Cards 3 1 2 3 4 5 6 7 8 Variable Type A1 F Default 0.0 O1 F 0.0 VARIABLE FID DESCRIPTION Function ID. Functions, tables , and load curves may not share common ID's. A unique number has to be defined. HEADING An optional descriptive heading. FUNCTION Function name. VARIABLE DESCRIPTION A1, A2, … Abscissa values. O1, O2, … Ordinate (function) values. Example: *BOUNDARY_PRESCRIBED_MOTION_SET $ function 300 prescribes z-acceleration of node set 1000 1000,3,1,300 *DEFINE_FUNCTION_TABULATED 201 tabfunc 0., 200 0.03, 2000. 1.0, 2000. *DEFINE_FUNCTION 300 a(t)=tabfunc(t)*t $$ following function is equivalent to one above for t < 0.03 $ a(t)=(200. + 60000.*t)*t *DEFINE_GROUND_MOTION Purpose: Define an earthquake ground motion history using ground motion records provided as load curves, for use in conjunction with *LOAD_SEISMIC_SSI for dynamic earthquake analysis including nonlinear soil-structure interaction. Card 1 1 2 3 4 5 6 7 8 Variable GMID ALCID VLCID Type I I Default none none I 0 VARIABLE DESCRIPTION GMID Ground motion ID. A unique number has to be defined. ALCID Load curve ID of ground acceleration history. VLCID Load curve ID of ground velocity history. Remarks: 1. Earthquake ground motion data is typically available either only as ground accelerations, or as a triple of ground accelerations, velocities and displace- ments. Usually, the velocities and the displacements are computed from the accelerations using specialized filtering and baseline correction techniques, e.g. see peer.berkeley.edu/smcat/process.html. Either input is accepted, with each quantity specified as a load curve. Only the acceleration and the velocity is required in the latter case; LS-DYNA does not require the ground displacement. 2. If only the ground acceleration data is provided for a particular ground motion, LS-DYNA generates a corresponding load curve for the velocity by integrating the acceleration numerically. The generated load curves are printed out to the D3HSP file. It is up to the user to ensure that these generated load curves are satisfactory for the analysis. *DEFINE Purpose: To model the heat affect zone in a welded structure, the yield stress and failure strain are scaled in shell models as a function of their distance from spot welds and the nodes specified in *DEFINE_HAZ_TAILOR_WELDED_BLANK. Card 1 1 2 3 4 5 6 7 8 Variable ID_HAZ IOP PID PID_TYP Type Default I 0 Card 2 1 I 0 2 I 0 3 I 0 4 Variable ISS IFS ISB IFB Type Default I 0 I 0 I 0 I 0 5 ISC I 0 6 IFC I 0 7 8 ISW IFW I 0 I 0 VARIABLE DESCRIPTION ID_HAZ Property set ID. A unique ID number must be used. IOP Activity flag. If IOP = 0, then the scaling is not applied, and if IOP = 1, the scaling is active. PID Part or part set ID. PID_TYP ISS PID type. PID_TYP = 0 indicates that PID is a *PART ID, and PID_TYP = 1, a part set. Curve ID for scaling the yield stress based on the distance to the closest solid element spot weld. Use a negative ID for curves normalized by the spot weld diameter as described in the Remarks below. *DEFINE_HAZ_PROPERTIES DESCRIPTION IFS ISB IFB ISC IFC ISW IFW Curve ID for scaling the failure strain based on the distance to the closest solid element spot weld. Use a negative ID for curves normalized by the spot weld diameter as described in the Remarks below. Curve ID for scaling the yield stress based on the distance to the closest beam element spot weld. Use a negative ID for curves normalized by the spot weld diameter as described in the Remarks below. Curve ID for scaling the failure strain based on the distance to the closest beam element spot weld. Use a negative ID for curves normalized by the spot weld diameter as described in the Remarks below. Curve ID for scaling the yield stress based on the distance to the closest constrained spot weld. Use a negative ID for curves normalized by the spot weld diameter as described in the Remarks below. Curve ID for scaling the failure strain based on the distance to the closest constrained spot weld. Use a negative ID for curves normalized by the spot weld diameter as described in the Remarks below. Curve ID for scaling the yield stress based on the distance to the closest tailor welded blank node. Use a negative ID for curves normalized by the spot weld diameter as described in the Remarks below. Curve ID for scaling the failure strain based on the distance to the tailor welded blank node. Use a negative ID for curves normalized by the spot weld diameter as described in the Remarks below. Remarks: The yield stress and failure strain are assumed to vary radially as a function of the distance of a point to its neighboring spot welds. Since larger spot welds may have a larger radius of influence, the smallest scale factor for the yield stress from all the neighboring spot welds is chosen to scale the yield stress at a particular point. The failure strain uses the scaling curve for the same weld. Curve IDs may be input as negative values to indicate that they are normalized by the diameter of the spot weld to compensate for the effects of the spot weld size. When this option is used, the scale factor is calculated based on the distance divided by the spot weld diameter for the spot weld that is closest to the element. The distance from a spot weld (or node for the blank) is measured along the surface of the parts in the part set. This prevents the heat softening effects of a weld from jumping across empty space. The HAZ capability only works with parts with materials using the STOCHASTIC option. It may optionally be simultaneously used with *DEFINE_STOCHASTIC_VARI- ATION to also account for the spatial variations in the material properties. See *DE- FINE_STOCHASTIC_VARIATION for more details. *DEFINE_HAZ_TAILOR_WELDED_BLANK Purpose: Specify nodes of a line weld such as in a Tailor Welded Blank. The yield stress and failure strain of the shell elements in the heat affected zone (HAZ) of this weld are scaled according to *DEFINE_HAZ_PROPERTIES. Card 1 1 2 3 4 5 6 7 8 Variable IDTWB IDNS Type Default I 0 I 0 VARIABLE DESCRIPTION IDTWB Tailor Welded Blank ID IDNS Node Set ID defining the location of the line weld. *DEFINE_HEX_SPOTWELD_ASSEMBLY_{OPTION} Purpose: Define a list of hexahedral elements that make up a single spot weld for computing the force and moment resultants that are written into the swforc output file. A maximum of 16 elements may be used to define an assembly representing a single spot weld. See Figure 15-45. This table of element IDs is generated automatically when beam elements are converted to solid elements. See the input parameter RPBHX associated with the keyword *CONTROL_SPOTWELD_BEAM. Available options for this command are: <BLANK> N For the <BLANK> option, all solid elements specified on Card 2 make up the spot weld and no additional card is read. For the N option, N is an integer representing the total number of solid elements making up the spot weld. If N is greater than 8, the additional card beyond Card 2 is read. N may not exceed 16. Card 1 1 2 3 4 5 6 7 8 Variable ID_SW Type Default I 0 Card 2 1 2 3 4 5 6 7 8 Variable EID1 EID2 EID3 EID4 EID5 EID6 EID7 EID8 Type Default I 0 I 0 I 0 I 0 I 0 I 0 I 0 I Figure 15-45. Illustration of four, eight, and sixteen element assemblies of solid hexahedron elements forming a single spot weld. Additional card for N > 8. Optional 1 2 3 4 5 6 7 8 Variable EID9 EID10 EID11 EID12 EID13 EID14 EID15 EID16 Type Default I 0 I 0 I 0 I 0 I 0 I 0 I 0 I 0 VARIABLE DESCRIPTION ID_SW Spot weld ID. A unique ID number must be used. EIDn Element ID n for up to 16 solid hexahedral elements. Remarks: The elements comprising a spot weld assembly may share a part ID (PID) with elements in other spot weld assemblies defined using *DEFINE_HEX_SPOTWELD_ASSEMBLY but may not share a PID or even a material ID (MID) with elements that are not included in a *DEFINE_HEX_SPOTWELD_ASSEMBLY. *DEFINE_LANCE_SEED_POINT_COORDINATES Purpose: The keyword is to activate the trimming in lancing. It is used in conjunction with *ELEMENT_LANCING to define a seed point which would be on the remaining part after lancing and trim. Card 1 1 Variable NSEED Type I Default none 2 X1 F 0 3 Y1 F 0 4 Z1 F 0 5 X2 F 0 6 Y2 F 7 Z2 F 0.0 0.0 8 VARIABLE DESCRIPTION NSEED Number of seed points. Maximum value of “2” is allowed. X1, Y1, Z1 Location coordinates of seed point #1. X2, Y2, Z2 Location coordinates of seed point #2. Remarks: 1. This keyword will remove all scraps during or after lancing, dependent on how the parameter AT is defined in *ELEMENT_LANCING. Lancing curves must form a closed loop, meaning first and last point coordinates must be coincident. Scraps are the portions that are exclusive of the portions whose seed points are defined by this keyword. 2. The following input defines two sets of seed point coordinates, where a double- attached part may be lanced and trimmed: *DEFINE_LANCE_SEED_POINT_COORDINATES $ NSEED X1 Y1 Z1 X2 Y2 Z2 2 -289.4 98.13 2354.679 -889.4 91.13 255.679 3. Refer to manual pages in *ELEMENT_LANCING for more details. Revision Information This feature is available in LS-DYNA Revision 107262 and later releases. : *DEFINE Purpose: To control the content of the history variables in the d3plot database. This feature is supported for solid, beam and shell elements. Define as many cards as needed to define the extra history variables. This input ends at the next keyword “*” card. Card 1 Variable Type Default 1 LABEL A40 none 2 A1 F 3 A2 F 4 A3 F 5 A4 F 0.0 0.0 0.0 0.0 VARIABLE DESCRIPTION LABEL String identifying history variable type. An Attributes, see discussion below. Remarks: Material models in LS-DYNA use history variables that are specific to the constitutive model being used. For most materials, 6 are reserved for the Cauchy stress components and 1 for the effective plastic strain, but many models have more than that. The history variables may include interesting physical quantities like material damage, material phase compositions, strain energy density and strain rate, but, in addition, they may also include nonphysical quantities like material direction cosines, scale factors and parameters that are used for the numerical algorithms but hard to interpret when post- processed. By using NEIPS, NEIPB and NEIPH on *DATABASE_EXTENT_BINARY, these extra history variables can be exported to the d3plot database in the order that they are stored, and in LS-PrePost the variables may then be plotted (Hist button) or fringed (Misc menu). There are a few drawbacks with this approach. The user must, for instance, have knowledge of the storage location of a certain history variable for a given material model and element type. While this information can be retrieved either in the LS- DYNA manual, on LS-DYNA support sites or in LS-PrePost itself, it is not always convenient. Furthermore, the same physical quantity may be stored in different locations for different materials and different element types, meaning that history variable #1 will correspond to different things in different parts which complicate post-processing of large models. The user may also be interested in a certain material specific quantity that is not necessarily stored as a history variable, this is not retrievable using this approach. Finally, if the history variable of interest happens to be stored in a bad location, i.e., among the last ones in a long list, it would be necessary to set NEIPS, NEIPB and/or NEIPH large enough to access this variable in LS-PrePost. This could result in unnecessarily large binary plot files. The present keyword is an attempt to organize the extra history variables with respect to uniformity, a goal is to get an output that is reasonably small and easy to interpret. The input is very simple, use the keyword *DEFINE_MATERIAL_HISTORIES in the keyword input deck, followed by lines that specify the history variables of interest using predetermined labels and attributes. NEIPS, NEIPB and NEIPH on *DATA- BASE_EXTENT_BINARY will then be overridden by the number of history variables, i.e., number of lines, requested on this card. As an example *DEFINE_MATERIAL_HISTORIES Instability Damage would mean that two extra history variables are output to the d3plot database, so NEIPS, NEIPB and NEIPH will internally be set to 2 regardless of the user input. History variable #1 will correspond to an instability measure (between 0 and 1) and history variable #2 will correspond to a material damage (between 0 and 1), i.e., the history variables are output in the order they are listed. If there are several instances of this keyword in an input deck, then the order of the history variables will follow the order that the cards are read by the keyword reader. In the d3hsp file the user may find the complete list by searching for the string “M a t e r i a l H i s t o r y L i s t”. For a material that does not store or calculate an “instability” or “damage” history variable, the output will be zero and thus the output will not be cluttered by unwanted data. Note that this keyword does not necessarily require that the history variable be stored, as long as it can be calculated when LS-DYNA outputs a plot state. This opens for the possibility to request quantities that are not available by just using NEIPS, NEIPB and/or NEIPH on *DATABASE_EXTENT_BINARY. For large models with many different parts and materials, the Instability or Damage variables should provide a comprehensive overview and understanding of the critical areas in terms of failure that otherwise may not be assessable. The permitted LABELs (case-sensitive) are Instability Damage A number between 0 and 1 that indicates how close a element or integration point is to failure or to initiate damage, no attributes apply to this label. A number between 0 and 1 indicating the damage level of the element or integration point, no attributes apply to this label. Plastic Strain Rate Effective plastic strain rate, calculated generically for “all” plastic materials from the evolution of effective plastic strain, no attributes apply to this label. History Fetch a history variable at a known place for a given material type, element type and part set. The following attributes apply. A1 A2 A3 A4 History variable location, mandatory. Material type, default applies to all materials. Element type, 0 for all element types, 1 for solids, 2 for shells and 3 for beams. Part set, history will only be fetched from the parts in the given part set. The default is all parts in the model. Examples: The History label is for users who know where history variables of interest are stored and want to use this to compress or simplify the output. An example is *DEFINE_MATERIAL_HISTORIES History,4,272,1,23 History,1,81 *SET_PART_LIST 23 2,3 which will make a list of two history variables in the output. History variable #1 will fetch the 4th history variable, but displayed only for the RHT concrete model (material 272), solid elements and in parts 2 and 3. History variable #2 will fetch the 1st history variable, display it only for the plasticity with damage model (material 81), but for any element and part. Both of these requested variables happen to be the damage in the respective materials, so an alternative to do something similar would be to use *DEFINE_MATERIAL_HISTORIES Damage for which the damage for all materials will be displayed in history variable #1. The history variables that may be requested using this keyword are tabulated in the individual material model chapters, see Volume II of the Keyword Users’ Manual. At the end of the remarks for a material model, a table such as the one below is present if there are retrievable history variables. *DEFINE_MATERIAL_HISTORIES Properties Label Attributes Description Instability Plastic Strain Rate - - - - - - - - 𝑝 , see FAIL Failure indicator 𝜀eff 𝑝 Effective plastic strain rate 𝜀̇eff 𝑝 /𝜀fail Whether mentioned in such table or not, Plastic Strain Rate is available for any material model that calculates plastic strain as the 7th standard history variable. Label in the table states what the string LABEL on *DEFINE_MATERIAL_HISTORIES must be, a1 to a4 will list attributes A1 to A4 if necessary, and Description will be a short description of what is output with this option, including possible restrictions. Further development of this keyword will mainly be driven by customer requests submitted to sugges- tions@lstc.com. Currently only solid, beam and shell elements are supported for the binary d3plot format, a goal is to include thick shells and support ascii/binout output in future versions of LS-DYNA. Note: The Labels are case-sensitive. *DEFINE_MULTI_DRAWBEADS_IGES Purpose: This keyword is developed to simplify the creation and definition of draw beads, which previously required the use of many keywords. Card 1 1 2 3 4 5 6 7 8 Variable Type Default FILENAME A80 none Card 2 1 2 3 4 5 6 7 8 Variable DBID VID PID BLKID NCUR Type I I Default none none I 1 I 1 I none IGES Curve ID cards. For multiple draw bead curves include as many cards as necessary. Input is terminated at the next (“*”) card. Card 3 1 2 3 4 5 6 7 8 Variable CRVID BFORCE Type I F Default none 0.0 VARIABLE DESCRIPTION DBID VID Draw bead set ID, which may consists many draw bead segments. Vector ID, as defined by *DEFINE_VECTOR. This vector is used to project the supplied curves to the rigid tool, defined by the parameter PID below. Part ID of a rigid tool to which the curves are projected and attached. Part ID of the blank. Number of draw bead curve segments (in the IGES file defined by FILENAME) to be defined. IGES curve ID for each segment. Draw bead force for each segment. *DEFINE VARIABLE PID BLKID NCUR CVRID BFORCE Remarks: 1. This keyword alone can be used to define draw bead forces around a stamping part. The following partial keyword example shows a draw bead set with ID 98, consists of three curves with ID, 12, 23, and 45, each with bead forces of 102.1, 203.3, 142.5 Newton/mm, respectively, are being created for blank with part ID 1. The beads are projected along vector ID 99, and are attached to a rigid tool with part ID 3. The IGES file to define the draw bead curve is “draw- beads3.iges”. *DEFINE_MULTI_DRAWBEADS_IGES drawbead3.iges $ DBID VID PID BLKID NCUR 98 99 3 1 3 $ CRVID BFORCE 12 102.1 23 203.3 45 142.5 *define_vector 99,0.0,0.0,0.0,0.0,0.0,1.0 Revision information: This feature is available in LS-DYNA R5 Revision 62840 and later releases. *DEFINE Purpose: To define a simple geometry for initial air domain. Card 1 1 2 3 4 5 6 7 8 Variable GID GTYPE1 GTYPE2 Type Default Card 2 Variable I 0 1 XA Type F Default 0. Card 3 Variable 1 X0 Type F Default 0. Card 4 Variable 1 XC Type F Default 0. I 0 2 YA F 0. 2 Y0 F 0. 2 YC F 0. I 0 3 ZA F 0. 3 Z0 F 0. 3 ZC F 0. 7 8 7 8 7 8 4 XB F 0. 4 G1 F 0. 4 G4 F 0. 5 YB F 0. 5 G2 F 0. 5 G5 F 0. 6 ZB F 0. 6 G3 F 0. 6 G6 F 0. VARIABLE DESCRIPTION GID ID of a GEOMETRY defining initial air particle domain. GTYPE1 GTYPE2 Geometry type EQ.1: box EQ.2: sphere EQ.3: cylinder EQ.4: ellipsoid EQ.5: hemisphere XA, YA, ZA (XA, YA, ZA) defines a vector of the 𝑥-axis XB, YB, ZB (XB, YB, ZB) defines a vector of the 𝑦-axis X0, Y0, Z0 Center coordinates of air domain G1 Dimension value depending on GTYPE. GTYPE.EQ.1: length of 𝑥 edge GTYPE.EQ.2: Radius of sphere GTYPE.EQ.3: Radius of cross section GTYPE.EQ.4: length of 𝑥-axes GTYPE.EQ.5: Radius of hemisphere G2 Dimension value depending on GTYPE. GTYPE.EQ.1: length of 𝑦 edge GTYPE.EQ.3: length of cylinder GTYPE.EQ.4: length of 𝑦-axes G3 Dimension value depending on GTYPE. GTYPE.EQ.1: length of 𝑧 edge GTYPE.EQ.4: length of 𝑧-axes XC, YC, ZC Center coordinates of domain excluded from the air domain G4, G5, G6 See definition of G1, G2, G3 *DEFINE 1. If GTYPE1/GTYPE2 is 5, the hemisphere is defined in negative 𝑧 direction defined by the cross product of the 𝑦 and 𝑥 axis. *DEFINE_PBLAST_GEOMETRY Purpose: To define a simple geometry for high explosives domain. Card 1 1 2 3 4 5 6 7 8 Variable GID GTYPE Type Default Card 2 Variable I 0 1 XA Type F Default 0. Card 3 Variable 1 Xc Type F Default 0. Card 4 Variable 1 G1 Type F Default 0. 15-212 (DEFINE) I 0 2 YA F 0. 2 Yc F 0. 2 G2 F 0. 3 ZA F 0. 3 Zc F 0. 3 G3 F 0. 7 8 4 XB F 0. 5 YB F 0. 6 ZB F 0. 4 5 6 7 8 4 5 6 VARIABLE DESCRIPTION GID ID of a GEOMETRY defining high explosive particle domain. GTYPE Geometry type EQ.1: box EQ.2: sphere EQ.3: cylinder EQ.4: ellipsoid EQ.5: hemisphere XA, YA, ZA (XA, YA, ZA) defines a vector of the x-axis XB, YB, ZB (XB, YB, ZB) defines a vector of the y-axis XC YC ZC G1 G2 G3 X-coordinate of charge center Y-coordinate of charge center Z-coordinate of charge center GTYPE.EQ.1: length of X edge GTYPE.EQ.2: Radius of sphere GTYPE.EQ.3: Radius of cross section GTYPE.EQ.4: length of X-axes GTYPE.EQ.5: Radius of hemisphere GTYPE.EQ.1: length of Y edge GTYPE.EQ.3: length of cylinder GTYPE.EQ.4: length of Y-axes GTYPE.EQ.1: length of Z edge GTYPE.EQ.4: length of Z-axes Remarks: 1. If GTYPE is 5, the hemisphere is defined in negative Z direction defined by the cross product of the Y and X axis. *DEFINE_PLANE Purpose: Define a plane with three non-collinear points. The plane can be used to define a reflection boundary condition for problems like acoustics. Card 1 1 Variable PID Type Default Card 2 Variable I 0 1 X3 Type F 2 X1 F 3 Y1 F 4 Z1 F 5 X2 F 6 Y2 F 7 Z2 F 0.0 0.0 0.0 0.0 0.0 0.0 4 5 6 7 2 Y3 F 3 Z3 F 8 CID I 0 8 Default 0.0 0.0 0.0 VARIABLE DESCRIPTION PID Plane ID. A unique number has to be defined. X1 Y1 Z1 X2 Y2 Z2 CID X-coordinate of point 1. Y-coordinate of point 1. Z-coordinate of point 1. X-coordinate of point 2. Y-coordinate of point 2. Z-coordinate of point 2. Coordinate system ID applied to the coordinates used to define the current plane. The coordinates X1, Y1, Z1, X2, Y2, Z2, X3, Y3 and Z3 are defined with respect to the coordinate system CID. X3 X-coordinate of point 3. VARIABLE DESCRIPTION Y3 Z3 Y-coordinate of point 3. Z-coordinate of point 3. Remarks: 1. The coordinates of the points must be separated by a reasonable distance and not collinear to avoid numerical inaccuracies. Available options include: ALE LAGRANGIAN *DEFINE_POROUS Purpose: The *DEFINE_POROUS_ALE card defines the Ergun porous coefficients for ALE elements. It is to be used with *LOAD_BODY_POROUS. This card with the LA- GRANGIAN option, the porous coefficients for Lagrangian elements and is to be used with *CONSTRAINED_LA- GRANGE_IN_SOLID (slave parts with CTYPE = 11 or 12). *DEFINE_POROUS_LAGRANGIAN, defines Card 1 1 2 3 4 5 6 7 8 Variable EIDBEG EIDEND LOCAL VECID1 VECID2 USERDEF Type I Default none Card 2 1 I 0 2 I 0 3 I 0 4 I 0 5 I 0 6 Variable Axx Axy Axz Bxx Bxy Bxz Type F F F F F F Default 0.0 0.0 0.0 0.0 0.0 0.0 7 8 Card 2 1 2 3 4 5 6 7 8 Variable Ayx Ayy Ayz Byx Byy Byz Type F F F F F F Default 0.0 0.0 0.0 0.0 0.0 0.0 Card 2 1 2 3 4 5 6 7 8 Variable Azx Azy Azz Bzx Bzy Bzz Type F F F F F F Default 0.0 0.0 0.0 0.0 0.0 0.0 VARIABLE EIDBEG, EIDEND DESCRIPTION EIDBEG, EIDEND > 0: EIDBEG, EIDEND < 0: Range of thick porous element IDs. These are solids in 3D and shells in 2D. Range of thin porous element IDs. These are shells in 3D and beams in 2D. The ALE option does not sup- port thin porous elements. EIDBEG > 0, EIDEND = 0: EIDBEG is a set of thick porous elements EIDBEG > 0, EIDEND < 0: EIDBEG is a set of thin porous elements LOCAL Flag to activate an element coordinate system: EQ.0: The forces are applied in the global directions. EQ.1: The forces are applied in a local system attached to the element. The system is consistent with DIREC = 1 and CTYPE = 12 in *CONSTRAINED_LAGRANGE_IN_SOL- ID. For CTYPE = 11, LOCAL is always 1 and the 𝑥-axis is aligned with the element normal while the 𝑦-axis passes through the element center and the first node in the ele- ment connectivity (*ELEMENT_BEAM in 2D or *ELE- MENT_SHELL in 3D) VECID1, VECID2 *DEFINE_POROUS DESCRIPTION *DEFINE_VECTOR IDs to define a specific coordinate system. VECID1 and VECID2 give the 𝑥- and 𝑦-direction respectively. The 𝑧-vector is a cross product of VECID1 and VECID2. If this latter is not orthogonal to VECID1, its direction will be corrected with a cross-product of 𝑧- and 𝑥-vectors. The vectors are stored as isoparametric locations to update their directions if the element deforms or rotates. USERDEF Flag to compute Aij and Bij with a user defined routine in the file dyn21.F called lagpor_getab_userdef. The file is part of the general package usermat. Viscous matrix for the porous flow Ergun equation. : Inertial matrix for the porous flow Ergun equation. : Aij Bij Remarks: 1. Ergun Equation. The Ergun equation computing the pressure gradient along each direction 𝑖 = 𝑥, 𝑦, 𝑧 can be written as follows: 𝑑𝑃 𝑑𝑥𝑖 = ∑[𝜇𝐴𝑖𝑗𝑉𝑗 + 𝜌𝐵𝑖𝑗∣𝑉𝑗∣𝑉𝑗] 𝑗=1 Where, a) 𝑉𝑖 is the relative velocity of the flow in the porous media b) 𝐴𝑖𝑗 are the viscous coefficients of the Ergun-type porous flow equation in the ith direction.. This matrix is similar to the viscous coefficients used in *LOAD_BODY_POROUS. c) 𝐵𝑖𝑗 are the inertial coefficient of the Ergun-type porous flow equation in the ith direction. This matrix is similar to the inertial coefficients used in *LOAD_BODY_POROUS. If this keyword defines the porous properties of Lagrangian elements in *CONSTRAINED_LAGRANGE_IN_SOLID, the porous coupling forces are computed with the pressure gradient as defined above instead of the equa- tions used for CTYPE = 11 and 12. *DEFINE Purpose: Defines a closed gas filled tube for the simulation of interior pressure waves that result from changes in the tube cross section area over time. The tube is defined by tubular beam elements, and the gas volume is determined by beam cross section area and initial element lengths. Area changes are given by contact penetration from surrounding elements (only mortar contacts currently supported). The pressure calculation is not coupled with the deformation of the beam elements and does not use any data from the material card. Pressure and tube area at the beam nodes are output through *DATABASE_PRTUBE. 4 5 6 7 8 Card 1 1 Variable PID Type Default I 0 Optional card 2 WS F 3 PR F 0.0 0.0 Card 2 1 2 3 4 5 6 7 8 Variable VISC CFL DAMP Type F F F Default 1.0 0.9 0.0 PID *DEFINE_PRESSURE_TUBE DESCRIPTION Part ID of tube. All connected beam elements in the part will model a closed tube. Only tubular beam elements are allowed, i.e. ELFORM = 1,4,5,11 with CST = 1 on *SECTION_BEAM. Initial tube cross section area is calculated using the beam inner diameter TT1/TT2. If no inner diameter is given, the outer diameter TS1/TS2 is used. The beam elements may not contain junctions and two different parts where *DEFINE_PRESSURE_TUBE is applied may not share nodes. For MPP all elements in the part will be on a single processor. WS PR VISC CFL Speed of sound 𝑐0 in the gas Initial gas pressure 𝑝0 inside tube Artificial viscosity multiplier 𝒗, see remarks CFL-factor 𝒌, see remarks DAMP Linear damping 𝒅, see remarks Remarks: The pressure tube is modeled with an acoustic approximation of the 1D compressible Euler equations for pipes with varying thickness 𝜕 𝜕𝑡 (𝜌𝐴) + 𝜕 𝜕𝑥 (𝜌𝑢𝐴) = 0, 𝜕 𝜕𝑡 (𝜌𝑢𝐴) + 𝜕 𝜕𝑡 (𝐸𝐴) + 𝜕 𝜕𝑥 𝜕 𝜕𝑥 (𝜌𝑢2𝐴 + 𝑝𝐴) = 𝑝 𝜕𝐴 𝜕𝑥 , (𝑢(𝐸 + 𝑝)𝐴) = 0, where 𝐴 = 𝐴(𝑥, 𝑡) is the cross section area and 𝜌, 𝑝, 𝑢, 𝐸 is density, pressure, velocity, and energy per unit volume, respectively. The above system is closed under the constitutive relations 𝐸 = 𝜌𝑒 + 𝜌𝑢2 , 𝑝 = 𝑝(𝜌, 𝑒), where 𝑒 is the internal energy per unit mass. For an isentropic and isothermal flow, the pressure will be proportional to the density, i.e. 𝑝 = 𝑐0 2𝜌, and the energy equation can be dropped. This is a good approximation of the Euler equations for acoustic flows where the state variables are smooth perturbations around a background state. For such flows no shocks will develop over time but may be present from initial/boundary values or source terms. Assuming small perturbations, linearization around (𝜌0, 𝑝0, 𝑢0 = 0) gives the acoustic approximation 𝜕𝑦 𝜕𝑥 𝜕 𝜕𝑡 𝜕𝑦 𝜕𝑡 (𝐴𝜌) + 𝜌0 2 𝜕 𝜕𝑥 + 𝑐0 𝜌0 (𝐴𝜌) = 𝑝 = 0, 𝜕𝐴 , 𝜕𝑥 where 𝑦 = 𝐴𝑢. Expressed in 𝑦 and 𝑝 we have 𝜕𝑝 𝜕𝑡 + 𝜕 ln 𝐴 𝜕𝑡 𝜕𝑦 𝜕𝑡 𝑝 + + 𝐴 𝑝0 𝑐0 𝑝0 𝜕𝑦 𝜕𝑥 𝜕𝑝 𝜕𝑥 = 0, = 0. This linearized system is solved using the standard Galerkin finite element method, using piecewise linear basis functions and artificial viscosity. Linear damping is added to model energy losses from friction between the gas and the tube walls. With artificial viscosity and linear damping, the system can be written as 𝜕𝑝 𝜕𝑡 + 𝜕 ln 𝐴 𝜕𝑡 𝜕𝑦 𝜕𝑡 𝑝 + + 𝐴 𝑝0 𝑐0 𝑝0 𝜕𝑦 𝜕𝑥 𝜕𝑝 𝜕𝑥 = 𝜖 = 𝜖 𝜕2𝑝 𝜕𝑥2 − 𝒅(𝑝 − 𝑝0) 𝜕2𝑦 𝜕𝑥2, where the artificial viscosity is proportional to the maximum initial beam element length, i.e. 𝜖 = 𝒗𝑐0 max Δ𝑥𝑖, Time integration is independent of the mechanical solver and uses a step size less than or equal to the global time step, satisfying a CFL condition Δ𝑡 < min 𝒌Δ𝑥𝑖 Δ𝑥𝑖 ∣𝜕 ln 𝐴 𝜕𝑡 ∣ + 3𝑐0 . *DEFINE_REGION Purpose: Define a volume of space, optionally in a local coordinate system. Card 1 Variable 1 ID Type I 2 3 4 5 6 7 8 TITLE A70 Card 2 1 2 3 4 5 6 7 8 Variable TYPE CID Type I I Card 3 for Rectangular Prism. Use when type = 0. Card 3 1 2 3 4 5 6 7 8 Variable XMN XMX YMN YMX ZMN ZMX Type F F F F F F Default 0.0 0.0 0.0 0.0 0.0 0.0 Card 3 for Sphere. Use when type = 1. Card 3 1 2 3 4 5 6 7 8 Variable XC1 YC1 ZC1 RMIN1 RMAX1 Type R R R R R Default 0.0 0.0 0.0 0.0 0.0 Card 3 for Cylinder. Use when type = 2. Card 3 1 2 3 4 5 6 7 8 Variable XC2 YC2 ZC2 AX2 AY2 AZ2 RMIN2 RMAX2 Type F F F F F F F F Default 0.0 0.0 0.0 0.0 0.0 0.0 0.0 0.0 Card 4 for Cylinder. Use when type = 2. 2 3 4 5 6 7 8 Card 4 Variable 1 L2 Type F Default 0.0 Card 3 for Ellipsoid. Use when type = 3. Card 3 1 2 3 4 5 6 7 8 Variable XC3 YC3 ZC3 AX3 AY3 AZ3 BX3 BY3 Type F F F F F F F F Default 0.0 0.0 0.0 0.0 0.0 0.0 0.0 0.0 Card 4 for Ellipsoid. Use when type = 3. Card 4 1 2 3 4 5 6 7 8 Variable BZ3 RA3 RB3 RC3 Type F F F F Default 0.0 0.0 0.0 0.0 VARIABLE DESCRIPTION ID TITLE TYPE CID XMN YMN ZMN XMX YMX ZMX Region ID Title for this region Region type: EQ.0: Box EQ.1: Sphere or spherical shell EQ.2: Cylinder or cylindrical shell, infinite or finite in length EQ.3: Ellipsoid Optional local coordinate system ID. If given, all the following input parameters will be interpreted in this coordinate system. Lower 𝑥 limit of box Lower 𝑦 limit of box Lower 𝑧 limit of box Upper 𝑥 limit of box Upper 𝑦 limit of box Upper 𝑧 limit of box XC1, YC1, ZC1 Coordinates of the center of the sphere RMIN1, RMAX1 The inner and outer radii of the spherical shell. Set RMIN1 = 0 for a solid sphere XC2, YC2, ZC2 A point on the cylindrical axis VARIABLE DESCRIPTION AX2, AY2, AZ2 A vector which defines the direction of the axis of the cylinder RMIN2, RMAX2 The inner and outer radii of the cylindrical shell. Set RMIN2 = 0 for a solid cylinder L2 Length of the cylinder. If L2 = 0, and infinite cylinder is defined. Otherwise the cylinder has one end at the point (XC2, YC2, ZC2) and the other at a distance L2 along the axis in the direction of the vector (AX2, AY2, AZ2) XC3, YC3, ZC3 Coordinates of the center of the ellipsoid AX3, AY3, AZ3 A vector in the direction of the first axis of the ellipsoid (axis 𝐚) BX3, BY3, BZ3 A vector, 𝐛̃ , in the plain of the first and second axes of the ellipsoid. The third axis of the ellipsoid (axis 𝐜) will be in the direction of 𝐚 × 𝐛̃ and finally the second axis 𝐛 = 𝐜 × 𝐚 RA3, RB3, RC3 The semi-axis lengths of the ellipsoid *DEFINE_SD_ORIENTATION Purpose: Define orientation vectors for discrete springs and dampers. These orientation vectors are optional for this element class. Four alternative options are possible. With the first two options, IOP = 0 or 1, the vector is defined by coordinates and is fixed permanently in space. The third and fourth option orients the vector based on the motion of two nodes, so that the direction can change as the line defined by the nodes rotates. Card 1 Variable VID Type Default I 0 Remarks none 2 IOP I 0 1 3 XT F 4 YT F 5 ZT F 0.0 0.0 0.0 6 7 8 NID1 NID2 I 0 I 0 IOP = 0,1 IOP = 0,1 IOP = 0,1 IOP = 2,3 IOP = 2,3 VARIABLE DESCRIPTION VID IOP Orientation vector ID. A unique ID number must be used. Option: EQ.0: deflections/rotations are measured and forces/moments applied along the following orientation vector. EQ.1: deflections/rotations are measured and forces/moments applied along the axis between the two spring/damper nodes projected onto the plane normal to the following orientation vector. EQ.2: deflections/rotations are measured and forces/moments applied along a vector defined by the following two nodes. EQ.3: deflections/rotations are measured and forces/moments applied along the axis between the two spring/damper nodes projected onto the plane normal to the a vector defined by the following two nodes. XT YT x-value of orientation vector. Define if IOP = 0,1. y-value of orientation vector. Define if IOP = 0,1. VARIABLE DESCRIPTION z-value of orientation vector. Define if IOP = 0,1. Node 1 ID. Define if IOP = 2,3. Node 2 ID. Define if IOP = 2, 3. ZT NID1 NID2 Remarks: 1. The orientation vectors defined by options 0 and 1 are fixed in space for the duration of the simulation. Options 2 and 3 allow the orientation vector to change with the motion of the nodes. Generally, the nodes should be members of rigid bodies, but this is not mandatory. When using nodes of deformable parts to define the orientation vector, care must be taken to ensure that these nodes will not move past each other. If this happens, the direction of the orien- tation vector will immediately change with the result that initiate severe insta- bilities can develop. *DEFINE_SET_ADAPTIVE Purpose: To control the adaptive refinement level by element or part set. Card 1 1 2 3 4 5 6 7 8 Variable SETID STYPE ADPLVL ADPSIZE Type I I I F Default none none none none VARIABLE DESCRIPTION SETID STYPE Element set ID or part set ID Set type for SETID: 1-element set 2-part set ADPLVL Adaptive refinement level for all elements in SETID set. ADSIZE Minimum element size to be adapted based on element edge length for all elements in SETID set. Remarks: 1. This option is for 3D-shell h-adaptivity only at the present time. 2. The order of defining refinement level for any elements is *CONTROL_ADAP- TIVE and *DEFINE_BOX_ADAPTIVE. 3. If there are multiple definitions of refinement level or element size for any elements, the latter one will be used. *DEFINE Purpose: The purpose of this keyword is to increase the efficiency of the SPH method’s neighborhood search algorithm by specifying an active region. All SPH elements located outside of the active region are deactivated. This card supports active regions consisting of the volume bounded by two closed surfaces (boxes, centered cylinders, and centered spheres are currently supported). Once the SPH particle is deactivated, it will stay inactive. Card 1 Variable 1 ID 2 3 4 5 6 7 8 TYPE STYPE CYCLE Type I Default none I 0 I 0 I 1 VARIABLE DESCRIPTION ID TYPE Part Set ID/Part ID EQ.0: Part set EQ.1: Part STYPE Type of the region. EQ.0: Rectangular box EQ.1: Cylinder EQ.2: Sphere CYCLE Number of cycles between each check Interior Rectangular Box Card. Card 2 format used for STYLE = 0. Card 2 1 2 3 4 5 6 7 8 Variable XIMIN YIMIN ZIMIN XIMAX YIMAX ZIMAX Type F F F F F F Default none none none none none none Outer Rectangular Box Card. Card 3 format used for STYPE = 0. Card 3 1 2 3 4 5 6 7 8 Variable XOMIN XOMIN ZOMIN XOMAX YOMAX ZOMAX Type F F F F F F Default none none none none none none VARIABLE XIMIN, YIMIN, ZIMIN XIMAX, YIMAX, ZIMAX XOMIN, YOMIN, ZOMIN XOMAX, YOMAX, ZOMAX DESCRIPTION Minimum x, y, z coordinate of the inner box Maximum x, y, z coordinates of the inner box Minimum x, y, z coordinate of the outer box Maximum x, y, z coordinates of the outer box Cylinder Axis Card. Card 2 format used for STYPE = 1. Card 2 Variable 1 X0 Type F 2 Y0 F 3 Z0 F 4 XH F 5 YH F 6 ZH F 7 8 Default none none none none none none Cylinder Radii Card. Card 3 format used for STYPE = 1. Card 3 1 2 3 4 5 6 7 8 Variable RMIN ZMIN RMAX ZMAX Type F F F F Default none none none none VARIABLE X0, Y0, Z0 DESCRIPTION Coordinates of the center of the cylinder base. The nested cylinders are sharing the same starting base plane. This point also serves as the tail for the vector specifying the direction of the cylinders’ axis. XH, YH, ZH Coordinates for the head of the cylinders axial direction vector. RMIN, ZMIN Radius and length of the interior cylinder. RMAX, ZMAX Radius and length of the outer cylinder. Center of Sphere Card. Card 2 used for STYPE = 2. 4 5 6 7 8 Card 2 Variable 1 X0 Type F 2 Y0 F 3 Z0 F Default none none none Sphere Radii Card. Card 3 used for STYPE = 2. Card 3 1 2 3 4 5 6 7 8 Variable RMIN RMAX Type F F Default none none VARIABLE DESCRIPTION X0, Y0, Z0 The spheres’ center. RMIN RMAX Radius of the interior sphere Radius of the outer sphere Remarks: 1.Cylindrical system for SPH active region Figure 15-46. Example DEFINE_SPH_ACTIVE_REGION *DEFINE_SPH_DE_COUPLING_{OPTION} Purpose: Define a penalty based contact. This option is to be used for the node to node contacts to couple SPH solver and discrete element sphere (DES) solver. The available options include: <BLANK> ID ID Card. Additional card for ID keyword option. Optional 1 2 3 4 5 6 7 8 Variable DID Type I Default none HEADING A80 none SPH Part Cards. Provide as many as necessary. Input ends at the next keyword (“*”) card. Card 1 1 2 3 4 5 6 7 8 Variable SPHID DESID SPHTYP DESTYP PFACT DFACT SPHBOX Type I I I I F F I Default none none none none 1.0 0. none VARIABLE DESCRIPTION DID Definition ID. This must be a unique number. HEADING Definition descriptor. It is suggested that unique descriptions be used. SPHID DESID SPH part or part set ID. DES part or part set ID. SPHTYP SPH part type: EQ.0: Part set ID, EQ.1: Part ID. DESTYP DES part type: EQ.0: Part set ID, EQ.1: Part ID. PFACT Penalty scale factor DFACT Penalty scale factor for contact damping coefficient SPHBOX BOX ID for SPH parts, See Remark 1. Remarks: SPHBOX is used to define the box IDs for the SPH parts. Only the particles that inside the boxes are defined for the node to node contacts. *DEFINE_SPH_INJECTION Purpose: This keyword injects SPH elements from user defined grid points. Card 1 1 2 3 Variable PID NSID CID Type I I I 4 VX F 5 VY F 6 VZ F 7 8 AREA F Default none none None 0.0 0.0 0.0 0.0 Card 2 1 2 3 4 5 6 7 8 Variable TBEG TEND Type F F Default 0.0 1.0E20 VARIABLE DESCRIPTION PID NSID CID Part ID of newly generated SPH elements. Node set ID. Nodes are used for initial injection position for the SPH elements. Local coordinate system ID, see *DEFINE_COORDINATE_SYS- TEM. X and Y coordinates define the injection plane, Z coordinate defines the normal to the injection plane. VX, VY, VZ Velocity of the inject elements: 𝐯 = (VX, VY, VZ) AREA TBEG TEND The area of initial injection surface. The density of injection flow comes from the material models see *MAT definition. Birth time Death time *DEFINE_SPH_TO_SPH_COUPLING_{OPTION} Purpose: Define a penalty based contact. This option is to be used for the node to node contacts between SPH parts. The available options include: <BLANK> ID ID Cards. Additional card for ID keyword option. Optional 1 2 3 4 5 6 7 8 Variable DID Type I Default none Sets of coupling cards: HEADING A70 none Each set consists of a Card 1 and may include an additional Card 2. Unless the card following Card 1 contains an “&” in its first column, the optional card is not read. Provide as many sets as necessary. This input terminates at the next keyword (“*”) card. Card 1 1 2 3 4 5 6 7 8 Variable SSID MSID SSTYP MSTYP IBOX1 IBOX2 PFACT SRAD Type I I I I I I F F Default none none none none none none 1.0 1.0 Optional. The keyword reader identifies this card by an “&” in the first column. Card 2 1 2 3 4 5 6 7 8 Variable DFACT ISOFT Type F Default 0.0 I 0 VARIABLE DESCRIPTION DID Definition ID. This must be a unique number. HEADING Definition descriptor. It is suggested that unique descriptions be used. SSID MSID Slave part or part set ID. Master part or part set ID. SSTYP Slave part type: EQ.0: Part set ID, EQ.1: Part ID. MSTYP Master part type: EQ.0: Part set ID, EQ.1: Part ID. IBOX1 IBOX2 Box ID for slave parts, See Remark 1. Box ID for master parts, See Remark 1. PFACT Penalty scale factor, See Remark 2. SRAD Scale factor for nodes to nodes contact criteria, See Remark 3. DFACT Penalty scale factor for contact damping coefficient, See Remark 4. Soft constraint option: EQ. 0: penalty formulation EQ. 1: soft constraint formulation The soft constraint may be necessary if the material constants of the parts in contact have a wide variation in the elastic bulk moduli. In the soft constraint option, the interface stiffness is based on the nodal mass and the global time step size. ISOFT Remarks: 1. IBOX1 and IBOX2 are used to define the box IDs for the slave parts and the master parts respectively. Only the particles that inside the boxes are defined for the node to node contacts. 2. For High Velocity Impact problems, a smaller value (ranges from 0.01 to 1.0e-4) of PFACT variable is recommended. A number ranges from 0.1 to 1 is recom- mended for low velocity contact between two SPH parts. 3. Contact between two SPH particles from different parts is detected when the distance of two SPH particles is less than SRAD*(sum of smooth lengths from two particles)/2.0. 4. DFACT = 0.0 is the default and is recommended. For DFACT > 0.0, interaction between SPH parts includes a viscous effect, providing some stickiness similar to the particle approximation invoked when CONT = 0 in *CONTROL_SPH. At present, no recommendation can be given for a value of DFACT other than the value should be less than 1.0. . *DEFINE_SPOTWELD_FAILURE_{OPTION} The available options are <BLANK> ADD Purpose: Define spot weld failure data for the failure criterion developed by Lee and Balur (2011). This is OPT = 10 on *MAT_SPOTWELD. It is available for spot welds consisting of beam elements, solid elements, or solid assemblies. Furthermore, *DE- FINE_SPOTWELD_FAILURE requires that the weld nodes be tied to shell elements using tied constraint based contact options: For beam element welds, only *CON- TACT_SPOTWELD is valid. For solid element welds or solid assembly welds, valid options are the following. *CONTACT_TIED_SURFACE_TO_SURFACE *CONTACT_SPOTWELD *CONTACT_TIED_SHELL_EDGE_TO_SURFACE Other tied contact types cannot be used. The ADD keyword option adds materials to a previously defined spot weld failure data set. Data Card 1. This card contains the data set’s ID and the first 7 parameters. When the ADD option is active leave the 7 parameters blank. Card 1 Variable 1 ID 2 3 4 5 6 7 8 TFLAG DC1 DC2 DC3 DC4 EXN EXS Type I Default none I 0 F F F F F F 1.183 0.002963 0.0458 0.1 1.51 1.51 Data Card 2. . This card contains 3 spot weld failure data parameters. Do not include this card when the ADD option is active Card 2 1 2 3 4 5 6 7 8 Variable NAVG D_SN D_SS R_SULT Type Default I 0 F F F none none 0.0 Material-Specific Strength Data Cards. Include one card for each material associated with the data set. The next keyword (“*”) card terminates the keyword. 4 5 6 7 8 Card 3 1 Variable MID Type I 2 SN F 3 SS F Default none none none VARIABLE DESCRIPTION ID Identification number of data set, input as FVAL on *MAT_- SPOTWELD TFLAG Thickness flag for nominal stress calculation EQ.0: Use minimum thickness EQ.1: Use average thickness Dynamic coefficient, 𝑐1 Dynamic coefficient, 𝑐2 Dynamic coefficient, 𝑐3 Dynamic coefficient, 𝑐4 Exponent on the normal term, 𝑛𝑛 Exponent on the shear term, 𝑛𝑠 DC1 DC2 DC3 DC4 EXN EXS *DEFINE_SPOTWELD_FAILURE DESCRIPTION NAVG Number of points in the time average of the load rates D_SN D_SS Default value of the static normal strength, 𝑆𝑛,stat Default value of the static shear strength, 𝑆𝑠,stat R_SULT Reference ultimate strength MID Material ID number of welded shell material Static normal strength of material MID. 𝑆𝑛,stat Static shear strength of material MID, 𝑆𝑠,stat SN SS Remarks: This stress based failure model, which was developed by Lee and Balur (2011), uses nominal stress in the numerator and dynamical strengths in the denominator. The weld fails when the stresses are outside of the failure surface defined as ( 𝑠𝑛 𝑆𝑛,dyn 𝑛𝑛 ) + ( 𝑠𝑠 S𝑠,dyn 𝑛𝑠 ) = 1 where 𝑠𝑛 and 𝑠𝑠 are nominal stress in the normal and tangential directions such that 𝑠𝑛 = 𝑠𝑠 = 𝑃𝑛 𝐷𝑡 𝑃𝑠 𝐷𝑡 . 𝑃𝑛 and 𝑃𝑠 are the loads carried by the weld in the normal and tangential directions, 𝐷is the weld diameter, and 𝑡 is the thickness of the welded sheets. If the sheets have different thicknesses, then TFLAG controls whether the minimum or average thickness is used. The dynamical strength terms in the denominator are load-rate dependent and are derived from static strength: 𝑆𝑛,dyn = 𝑆𝑛,stat [𝑐1 + 𝑐2 ( ) + 𝑐3 log ( )] 𝑆𝑠,dyn = 𝑆𝑠,stat [𝑐1 + 𝑐2 ( ) + 𝑐3log ( )] 𝑃̇𝑛 𝑐4 𝑃̇𝑠 𝑐4 𝑃̇𝑛 𝑐4 𝑃̇𝑠 𝑐4 where the constants 𝑐1 to 𝑐4 are the input in the fields DC1 to DC4, 𝑃̇𝑛 and 𝑃̇𝑠 are the load rates, and 𝑆𝑛,stat and 𝑆𝑠,stat are the static strengths of the welded sheet materials which for each material are input using SN and SS. When two different materials are welded, the material having the smaller normal strength determines the strengths used for the weld. Materials that do not have SN and SS values default to D_SN and D_SS from card 1. The default values for DC1 to DC4, and EXN and EXS are based on the work Chao, Wang, Miller and Zhu (2010). and Wang, Chao, Zhu, and Miller (2010). These parameters are unitless except for DC4 which has units of force per unit time. The default value of 0.1 is for MN/sec. The load rate, 𝑃̇, can be time averaged to reduce the effect of high frequency oscillations on the dynamic weld strength. NAVG is the number of terms in the time average. If R_SULT is defined on Card 2 and the PID keyword option is not used, then D_SN and D_SS are interpreted to be reference values of the normal and shear static strength, and the SN field on Card 3 is interpreted as a material specific ultimate strength. These values are then use to calculate material specific strength values by 𝑆𝑛,𝑠𝑡𝑎𝑡 = 𝑆𝑛,𝑟𝑒𝑓 ( 𝑆𝑢 𝑆𝑢,𝑟𝑒𝑓 ) 𝑆𝑠,𝑠𝑡𝑎𝑡 = 𝑆𝑠,𝑟𝑒𝑓 ( 𝑆𝑢 𝑆𝑢,𝑟𝑒𝑓 ) where 𝑆𝑛,𝑟𝑒𝑓 , 𝑆𝑠,𝑟𝑒𝑓 , and 𝑆𝑢,𝑟𝑒𝑓 , are D_SN, D_SS, and R_SULT on card 2, and 𝑆𝑢 is SN on card 3. With this option, the SS values are ignored. If the PID keyword option is used, then R_SULT is ignored and SN and SS are the static strength values. *DEFINE_SPOTWELD_FAILURE_RESULTANTS Purpose: Define failure criteria between part pairs for predicting spot weld failure. This table is implemented for solid element spot welds, which are used with the tied, constraint based, contact option: *CONTACT_TIED_SURFACE_TO_SURFACE. Note that other tied contact types cannot be used. The input in this section continues until then next “*” card is encountered. Default values are used for any part ID pair that is not defined. Only one table can defined. See *MAT_SPOTWELD where this option is used whenever OPT = 7. Card 1 Variable Type Default 1 ID I 0 2 3 4 5 6 7 8 DSN DSS DLCIDSN DLCIDSS F F 0.0 0.0 I 0 I 0 Failure Cards. Provide as many as necessary. The next keyword (“*”) card terminates the table definition. Card 2… 1 2 3 4 5 6 7 8 Variable PID_I PID_J SNIJ SSIJ LCIDSNIJ LCIDSSIJ Type I I F F Default none none 0.0 0.0 I 0 I 0 VARIABLE DESCRIPTION ID DSN DSS DLCIDSN Identification number. Only one table is allowed. Default value of the normal static stress at failure. Default value of the transverse static stress at failure. Load curve ID defining a scale factor for the normal stress as a function of strain rate. This factor multiplies DSN to obtain the failure value at a given strain rate. DESCRIPTION Load curve ID defining a scale factor for static shear stress as a function of strain rate. This factor multiplies DSN to obtain the failure value at a given strain rate. Part ID I. Part ID J. The maximum axial stress at failure between parts I and J. The axial stress is computed from the solid element stress resultants, which are based on the nodal point forces of the solid element. The maximum shear stress at failure between parts I and J. The shear stress is computed from the solid element stress resultants, which are based on the nodal point forces of the solid element. Load curve ID defining a scale factor for the normal stress as a function of strain rate. This factor multiplies SNIJ to obtain the failure value at a given strain rate. Load curve ID defining a scale factor for static shear stress as a function of strain rate. This factor multiplies SSIJ to obtain the failure value at a given strain rate. VARIABLE DLCIDSS PID_I PID_J SNIJ DSSIJ LCIDSNIJ LCIDSSIJ Remarks: The stress based failure model, which was developed by Toyota Motor Corporation, is a function of the peak axial and transverse shear stresses. The entire weld fails if the stresses are outside of the failure surface defined by: ( 𝜎𝑟𝑟 𝐹 ) 𝜎𝑟𝑟 + ( 𝜏𝐹) − 1 = 0 𝐹 and 𝜏𝐹 are specified in the above table by part ID pairs. LS-DYNA where 𝜎𝑟𝑟 automatically identifies the part ID of the attached shell element for each node of the spot weld solid and checks for failure. If failure is detected the solid element is deleted from the calculation. If the effects of strain rate are considered, then the failure criteria becomes: 𝜎𝑟𝑟 [ 𝐹 ] 𝑓𝑑𝑠𝑛(𝜀̇𝑝)𝜎𝑟𝑟 + [ 𝑓𝑑𝑠𝑠(𝜀̇𝑝)𝜏𝐹] − 1 = 0 *DEFINE_SPOTWELD_MULTISCALE Purpose: Associate beam sets with multi-scale spot weld types for modeling spot weld failure via the multi-scale spot weld method. Spot Weld/Beam Set Association Cards. Provide as many cards as necessary. This input ends at the next keyword (“*”) card. Card 1 1 2 3 4 5 6 7 8 Variable TYPE BSET TYPE BSET TYPE BSET TYPE BSET Type I I I I I I I I Default none none none none none none none none VARIABLE DESCRIPTION MULTISCALE spot weld type to use. SPOTWELD_MULTISCALE See *INCLUDE_- Beam set which uses this multi-scale spot weld type for failure modeling. TYPE BSET Remarks: See *INCLUDE_MULTISCALE_SPOTWELD for a detailed explanation of capability. this *DEFINE_SPOTWELD_RUPTURE_PARAMETER Purpose: Define a parameter by part ID for shell elements attached to spot weld beam elements using the constrained contact option: *CONTACT_SPOTWELD. This table will not work with other contact types. Only one table is permitted in the problem definition. Data, which is defined in this table, is used by the stress based spot weld failure model developed by Toyota Motor Corporation. See *MAT_SPOTWELD where this option is activated by setting the parameter OPT to a value of 9. This spot weld failure model is a development of Toyota Motor Corporation. Card 1 1 2 3 4 5 6 7 8 Variable PID Type I Default Card 2 1 2 3 4 5 6 7 8 Variable C11 C12 C13 N11 N12 N13 SIG_PF Type F F F F F F F Default Card 3 1 2 3 Variable C21 C22 C23 Type F F F 4 N2 F Default 5 6 7 8 SIG_NF Card 4 1 2 3 4 5 6 7 8 Variable LCDPA LCDPM LCDPS LCDNA LCDNM LCDNS NSMT Type Default I 0 I 0 I 0 I 0 I 0 I 0 I 0 VARIABLE DESCRIPTION PID Part ID for the attached shell. C11-N2 Parameters for model, see Remarks below. Nugget pull-out stress, σP. Nugget fracture stress, σF. Curve ID defining dynamic scale factor of spot weld axial load rate for nugget pull-out mode. Curve ID defining dynamic scale factor of spot weld moment load rate for nugget pull-out mode. Curve ID defining dynamic scale factor of spot weld shear load rate for nugget pull-out mode. Curve ID defining dynamic scale factor of spot weld axial load rate for nugget fracture mode. Curve ID defining dynamic scale factor of spot weld moment load rate for nugget fracture mode. Curve ID defining dynamic scale factor of spot weld shear load rate for nugget fracture mode. The number of time steps used for averaging the resultant rates for the dynamic scale factors. SIG_PF SIG_NF LCDPA LCDPM LCDPS LCDNA LCDNM LCDNS NSMT Remarks: This failure model incorporates two failure functions, one for nugget pull-out and the other for nugget fracture. The nugget pull-out failure function is 𝐹𝑝 = C11× 𝐴 𝐷N12 + C13 × 𝑆 𝐷N13 𝐷N11 + C12× 𝑀 𝜎𝑃 [1 + (𝜀̇𝑝 𝑝⁄ ] ) where A, M, and S are the axial force, moment, and shear resultants respectively, D is the spot weld diameter, and the Cowper-Symonds coefficients are from the attached shell material model. If the Cowper-Symonds coefficients aren’t specified, the term within the square brackets, [ ], is 1.0. The fracture failure function is 𝐹𝑛 = √(C21 × 𝐴 + C22 × 𝑀)2 + 3(C23 × 𝑆)2 𝐷N2𝜎𝐹 [1 + (𝜀̇𝑝 ) 𝑝⁄ ] . When the load curves for the rate effects are specified, the failure criteria are C11 × 𝑓dpa(𝐴̇) × 𝐴 𝐷N11 + 𝐶12 × 𝑓dpa(𝑀̇ ) × 𝑀 𝐷N12 + C13 × 𝑓dpa(𝑆̇) × 𝑆 𝐷N13 𝜎𝑃 √[C21 × 𝑓dna(𝐴̇) × 𝐴 + C22 × 𝑓dnm(𝑀̇ ) × 𝑀] + 3[C23 × 𝑓𝑑𝑛𝑠(𝑆̇) × 𝑆] 𝐷N2𝜎𝐹 𝐹𝑝 = 𝐹𝑛 = where f is the appropriate load curve scale factor. The scale factor for each term is set to 1.0 for when no load curve is specified. No extrapolation is performed if the rates fall outside of the range specified in the load curve to avoid negative scale factors. A negative load curve ID designates that the curve abscissa is the log10 of the resultant rate. This option is recommended when the curve data covers several orders of magnitude in the resultant rate. Note that the load curve dynamic scaling replaces the Cowper-Symonds model for rate effects. Failure occurs when either of the failure functions is greater than 1.0. *DEFINE_SPOTWELD_RUPTURE_STRESS Purpose: Define a static stress rupture table by part ID for shell elements connected to spot weld beam elements using the constrained contact option: *CONTACT_- SPOTWELD. This table will not work with other contact types. Only one table is permitted in the problem definition. Data, which is defined in this table, is used by the stress based spot weld failure model developed by Toyota Motor Corporation. See *MAT_- SPOTWELD where this option is activated by setting the parameter OPT to a value of 6. Part Cards. Define rupture stresses part by part. The next keyword (“*”) card terminates this input. Card 1 2 3 4 5 6 7 8 Variable PID SRSIG SIGTAU ALPHA Type I F F F VARIABLE DESCRIPTION PID SRSIG Part ID for the attached shell. 𝐹 . Axial (normal) rupture stress, 𝜎𝑟𝑟 SRTAU Transverse (shear) rupture stress, 𝜏𝐹. ALPHA Scaling factor for the axial stress as defined by Toyota. The default value is 1.0. Remarks: The stress based failure model, which was developed by Toyota Motor Corporation, is a function of the peak axial and transverse shear stresses. The entire weld fails if the stresses are outside of the failure surface defined by: ( 𝜎𝑟𝑟 𝐹 ) 𝜎𝑟𝑟 + ( 𝜏𝐹) − 1 = 0 𝐹 and 𝜏𝐹 are specified in the above table by part ID. LS-DYNA automatically where 𝜎𝑟𝑟 identifies the part ID of the attached shell element for each node of the spot weld beam and independently checks each end for failure. If failure is detected in the end attached to the shell with the greatest plastic strain, the beam element is deleted from the calculation. If the effects of strain rate are considered, then the failure criteria becomes: [ 𝜎𝑟𝑟 ] 𝐹 (𝜀̇𝑝) 𝜎𝑟𝑟 + [ ] 𝜏𝐹(𝜀̇𝑝) − 1 = 0 𝐹 (𝜀̇𝑝) and 𝜏𝐹(𝜀̇𝑝) are found by using the Cowper and Symonds model which where 𝜎𝑟𝑟 scales the static failure stresses: 𝜎𝑟𝑟 𝐹 (𝜀̇𝑝) = 𝜎𝑟𝑟 𝜀̇𝑝 ⎡1 + ( ⎢ ⎣ 𝑝⁄ ) ⎤ ⎥ ⎦ 𝑝⁄ 𝜀̇𝑝 𝜏𝐹(𝜀̇𝑝) = 𝜏𝐹 ⎡1 + ( ⎢ ⎣ where 𝜀̇𝑝is the average plastic strain rate which is integrated over the domain of the attached shell element, and the constants p and C are uniquely defined at each end of the beam element by the constitutive data of the attached shell. The constitutive model is described in the material section under keyword: *MAT_PIECEWISE_LINEAR_- PLASTICITY. ⎤ ⎥ ⎦ ) The peak stresses are calculated from the resultants using simple beam theory. 𝜎𝑟𝑟 = 𝑁𝑟𝑟 + √𝑀𝑟𝑠 2 + 𝑀𝑟𝑡 𝛼𝑍 𝜏 = 𝑀𝑟𝑟 2𝑍 + 2 + 𝑁𝑟𝑡 √𝑁𝑟𝑠 where the area and section modulus are given by: 𝐴 = 𝜋 𝑍 = 𝜋 𝑑2 𝑑3 32 and d is the diameter of the spot weld beam. *DEFINE_STAGED_CONSTRUCTION_PART_{OPTION} Available options include: <BLANK> SET Purpose: Staged construction. This keyword offers a simple way to define parts that are removed (e.g., during excavation), added (e.g., new construction) and used temporarily (e.g., props) during the analysis. Available for solid, shell, and beam element parts. Part Cards. Provide as many as necessary. This input ends at the next keyword (“*”) card. Card 1 1 2 3 4 5 6 7 8 Variable PID/PSID STGA STGR Type I I I Default none See Remark s See Remark s VARIABLE DESCRIPTION Part ID (or Part Set ID for the_SET option) Construction stage at which part is added Construction stage at which part is removed PID STGA STGR Remarks: Used with *DEFINE_CONSTRUCTION_STAGES (defines the meaning of stages STGA and STGR) and *CONTROL_STAGED_CONSTRUCTION. If STGA = 0, the part is present at the start of the analysis. If STGR = 0, the part is still present at the end of the analysis. Examples: 1. Soil that is excavated would have STGA = 0 but STGR > 0 2. New construction would have STGA > 0 and STGR = 0 3. Temporary works would have STGA > 0, STGR > STGA. This is a convenience feature that reduces the amount of input data needed for many typical construction models. Internally, LS-DYNA checks for *LOAD_REMOVE_PART, *LOAD_GRAVITY_PART and *LOAD_STIFFEN_PART referencing the same PID. Generally, these will not be present and LS-DYNA creates the data using STGA and STGR, and default gravity and pre-construction stiffness factor from *CONTROL_- STAGED_CONSTRUCTION. If existing cards are found, STGA and STGR are inserted into the existing data. During the analysis, any load curves entered on those existing cards will override STGA and STGR. *DEFINE_STOCHASTIC_ELEMENT_OPTION Options: SOLID_VARIATON for solid elements. SHELL_VARIATION for shell elements. Purpose: Define the stochastic variation in the yield stress, damage/failure models, density, and elastic moduli for solid material models with the STOCHASTIC option, currently materials 10, 15, 24, 81, and 98. This option overrides values assigned by *DE- FINE_STOCHASTIC_VARIATION. Card 1 1 2 3 4 5 6 7 8 Variable IDE VARSY VARF VARRO VARE Type Default I 0 F 0 F 0 F 0 F 0 VARIABLE DESCRIPTION IDE Element ID VARSY VARF VARRO VARE The yield stress and its hardening function are scaled by 1.+VARSY. The failure criterion is scaled by 1+VARF The density is scaled by 1+VARRO. This is intended to be used with topology optimization. This option is not available for shell elements. The elastic moduli are scaled by 1+VARE. This is intended to be used with topology optimization. *DEFINE_STOCHASTIC_VARIATION Purpose: Define the stochastic variation in the yield stress and damage/failure models for material models with the STOCHASTIC option, currently materials 10, 15, 24, 81, and 98 and the shell version of material 123. Card 1 1 2 3 4 5 6 7 8 Variable ID_SV PID PID_TYP ICOR VAR_S VAR_F IRNG Type Default I 0 I 0 I 0 I 0 I 0 I 0 I 0 Yield Stress Card for Built-in Distribution. Card 2 for VAR_S set to 0, 1, or 2. 4 5 6 7 8 Card 2 Variable 1 R1 Type F 2 R2 F 3 R3 F Default Yield Stress Card for Load Curve. Card 2 for VAR_S set to 3 or 4. Card 2 1 2 3 4 5 6 7 8 Variable LCID Type Default I Failure Strain Card for Built-in Distribution. Card 2 for VAR_F set to 0, 1, or 2. 4 5 6 7 8 Card 2 Variable 1 R1 Type F 2 R2 F 3 R3 F Default Failure Strain Card for Load Curve. Card 2 for VAR_F set to 3 or 4. Card 2 1 2 3 4 5 6 7 8 Variable LCID Type Default I 0 VARIABLE DESCRIPTION ID_SV Stochastic variation ID. A unique ID number must be used. PID *PART ID or *SET_PART ID. PID_TYP Flag for PID type. If PID and PID_TYP are both 0, then the properties defined here apply to all shell and solid parts using materials with the STOCHASTIC option. EQ.0: PID is a *PART ID. EQ.1: PID is a *SET_PART ID ICOR Correlation between the yield stress and failure strain scaling. EQ.0: Perfect correlation. EQ.1: No correlation. The yield stress and failure strain are independently scaled. VARIABLE DESCRIPTION VAR_S Variation type for scaling the yield stress. EQ.0: The scale factor is 1.0 everywhere. EQ.1: The scale factor is random number in the uniform random distribution in the interval defined by R1 and R2. EQ.2: The scale factor is a random number obeying the Gaussian distribution defined by R1, R2, and R3. EQ.3: The scale factor is defined by the probability distribution function defined by curve LCID. EQ.4: The scale factor is defined by the cumulative distribution function defined by curve LCID. VAR_F Variation type for scaling failure strain. EQ.0: The scale factor is 1.0 everywhere. EQ.1: The scale factor is random number in the uniform random distribution in the interval defined by R1 and R2. EQ.2: The scale factor is a random number obeying the Gaussian distribution defined by R1, R2, and R3. EQ.3: The scale factor is defined by the probability distribution function defined by curve LCID. EQ.4: The scale factor is defined by the cumulative distribution function defined by curve LCID. IRNG Flag for random number generation. EQ.0: Use deterministic (pseudo-) random number generator. The same input always leads to the same distribution. EQ.1: Use non-deterministic (true) random number generator. With the same input, a different distribution is achieved in each run. R1, R2, R3 Real values to define the stochastic distribution. See below. LCID Curve ID defining the stochastic distribution. See below. *DEFINE_STOCHASTIC_VARIATION Each integration point 𝑥𝑔 in the parts specifed by PID is assigned the random scale factors 𝑅𝑆 and 𝑅𝐹 that are applied to the values calculated by the material model for the yield stress and failure strain. 𝜎𝑦 = 𝑅𝑠(𝑥𝑔)𝜎𝑦(𝜀̅𝑝, … ) 𝜀̅FAIL = 𝑅𝐹(𝑥𝑔)𝜀̅FAIL (𝜀̇, 𝜀̅𝑝, … ) The scale factors vary spatially over the model according to the chosen statistical distributions defined in this section and are independent of time. The scale factors may be completely correlated or uncorrelated with the default being completely correlated since the failure strain is generally reduced as the yield stress increases. The scale factors 𝑅𝑆 and 𝑅𝐹 may be stored as extra history variables as follows: Material Model 10 15 24 81 98 123 (shells only) History Variable # for RS 5 7 6 6 7 6 History Variable # for RF 6 8 7 7 8 7 The user is responsible for defining the distributions so that they are physically meaningful and are restricted to a realistic range. Since neither the yield stress nor the failure strain may be negative, for example, the minimum values of the distributions must always be greater than zero. The probability that a particular value 𝑅 will occur defines the probability distribution function, 𝑃(𝑅). Since a value must be chosen from the distribution, the integral from the minimum to the maximum value of 𝑅 of the probability distribution function must be 1.0, 𝑅MAX ∫ 𝑅MIN 𝑃(𝑅)𝑑𝑅 = 1 . Another way to characterize a distribution is the cumulative distribution function 𝐶(𝑅) which defines the probability that a value will lie between 𝑅𝑀𝐼𝑁 and 𝑅, 𝐶(𝑅) = ∫ 𝑅MIN 𝑃(𝑅̂ )𝑑𝑅̂ . By definition 𝐶(𝑅𝑀𝐼𝑁) = 0 and 𝐶(𝑅𝑀𝐴𝑋) = 1. An inverse cumulative probability function D gives the number for a cumulative probability of 𝐶(𝑅), 𝐷(𝐶(𝑅)) = 𝑅. A random varriable satisfying the probability distribution function P(R) can be generated from a sequence of uniformly distributed numbers, 𝑅̂ 𝐼, for 𝐼 = 1, 𝑁, using the inverse cumulative distribution function 𝐷 as 𝑅𝐼 = 𝐷(𝑅̂ 𝐼). The scale factors for the yield stress and the failure strain may be generated using the same value of 𝑅̂ 𝐼 for both (ICOR = 0) or by using independent values each one (ICOR = 1). If the same values are used, there is perfect correlation, and the failure strain scale factor becomes an implicit value of yield stress scale factor. VAR = 0. No Scaling. The corresponding yield stress or failure strain is not scaled. VAR = 1. Scaling from Uniform Distribution A uniform distribution is specified by setting VAR = 1. The input variable R1 is interpreted as 𝑅MIN and R2 as 𝑅MAX. If R1 = R2, then the yield stress or failure strain will be scaled by R1. When using the uniform random distribution, the probability of a particular value is given by and the cumulative probability function is given by 𝑃(𝑅) = 𝑅MAX − 𝑅MIN 𝐶(𝑅) = 𝑅 − 𝑅MIN 𝑅MAX − 𝑅MIN . VAR = 2. Gaussian Distribution The Gaussian distribution, VAR = 2, is smoothly varying with a peak at µ and 63 percent of the values occurring within the interval of one standard deviation 𝜎, [𝜇 − 𝜎, 𝜇 + 𝜎]. The input parameter R1 is interpreted as the mean, 𝜇,, while R2 is interpreted as the standard deviation, 𝜎. There is a finite probability that the values of 𝑅 will be outside of the range that are physically meaningful in the scaling process, and R3 which is interpreted as 𝛿 restricts the range of R to [𝜇 − 𝛿, 𝜇 + 𝛿] The resulting truncated Gaussian distribution is rescaled such that, 𝐷(𝜇 + 𝛿) = 1. VAR = 3 or 4. Distribution from a Load Curve The user may directly specify the probability distribution function or the cumulative probability distribution function with *DEFINE_CURVE by setting VAR = 3 or VAR = 4, respectively, and then specifying the required curve ID on the next data card. Stochastic variations may be used simultaneously with the heat affected zone (HAZ) options in LS-DYNA . The effect of the scale factors from stochastic variation and HAZ options are multiplied together to scale the yield stress and failure strain, 𝜎𝑦 = 𝑅𝑆(𝑥𝑔)𝑅𝑆 𝜀̅FAIL = 𝑅𝐹(𝑥𝑔)𝑅𝐹 HAZ𝜎𝑦(𝜀̅𝑝, … ) HAZ𝜀̅FAIL (𝜀̇, 𝜀̅𝑝, … ). *DEFINE Purpose: To interpolate from point data a continuously indexed family of nonintersect- ing curves. The family of curves, ℱ , consists of x-y curves, 𝑓𝑠(𝑥), indexed by a parameter, 𝑠. ℱ = {𝑓𝑠(𝑥)∣∀𝑠 ∈ [𝑠min, 𝑠max]}. The interpolation is built up by sampling functions in ℱ at discrete parameter values, 𝑠𝑖, 𝑓𝑠𝑖(𝑥) ∈ ℱ . The points, 𝑠𝑖, are input to LS-DYNA on the data cards for the *DEFINE_TABLE keyword. LS-DYNA requires that they be ordered from least to greatest. The curves, 𝑓𝑠𝑖(𝑥), must be defined as lists of (𝑥, 𝑦) pairs in a collection of *DEFINE_CURVE sections that directly follow the *DEFINE_TABLE section. Each *DEFINE_CURVE section is paired to its corresponding 𝑠𝑖 value by list position (and not load curve ID, for that see *DEFINE_TABLE_2D). Card 1 1 2 3 4 5 6 7 8 Variable TBID SFA OFFA Type I F Default none 1. F 0. Points Cards. Place one point per card. The values must be in ascending order. Input is terminated when a “*DEFINE_CURVE” keyword card is found. Card 2 1 2 3 4 5 6 7 8 Variable VALUE Type F Default 0.0 Include one *DEFINE_CURVE input section here for each point defined above. The 𝑖th *DEFINE_CURVE card contains the curve at the 𝑖th *DEFINE_TABLE value. TBID *DEFINE_TABLE DESCRIPTION Table ID. Tables and Load curves may not share common ID's. LS-DYNA allows load curve ID's and table ID's to be used interchangeably. SFA Scale factor for VALUE. OFFA Offset for VALUE, see explanation below. VALUE Load curve will be defined corresponding to this value, e.g., this value could be a strain rate, see purpose above. Motivation: This capability was implemented with strain-rate dependent stress-strain relations in mind. To define such a function, the first step is to tabulate stress-strain curves at known strain-rate values. Then, the list of strain-rates is written in ascending order to the data cards following *DEFINE_TABLE. Following *DEFINE_TABLE, the tabulated stress-strain curves must be input to LS-DYNA as a set of *DEFINE_CURVE sections ordered so that the 𝑖th curve corresponds to the 𝑖th strain-rate point. This section is structured as: *DEFINE_TABLE strain-rate point 1 strain-rate point 2 ⋮ strain-rate point n *DEFINE_CURVE [stress-strain curve at strain-rate 1] *DEFINE_CURVE [stress-strain curve at strain-rate 2] ⋮ *DEFINE_CURVE [stress-strain curve at strain-rate n] Details, Features and Limitations: 1. All the curves in a table must start from the same abscissa value and end at the same abscissa value. This limitation is necessary to avoid slow indirect ad- dressing in the inner loops used in the constitutive model stress evaluation. Curves must not intersect except at the origin and end points. 2. Each curve may have unique spacing and an arbitrary number of points in its definition. 3. All the curves in a table must share the same value of LCINT. 4. In most applications, curves can only be extrapolated in one direction, that is, to the right of the last data point. An example would be curves representing effec- tive stress vs. effective plastic strain. For cases when extrapolation is only to the right, the curves comprising a table are allowed to intersect only at their starting point but the curves and their extrapolations must not intersect else- where. For other applications in which the curves are extrapolated in both directions, the curves and their extrapolations are not allowed to intersect except at the origin (0,0). An example would be curves representing force vs. change in gage length where negative values are compressive and positive values are tensile. 5. Load curve IDs defined for the table may be referenced elsewhere in the input. 6. No keyword commands may come between *DEFINE_TABLE and the *DE- FINE_CURVE commands that feed the table. The set of *DEFINE_CURVE commands must not be interrupted by any other keyword. This coupling be- tween *DEFINE_TABLE and subsequent *DEFINE_CURVE commands is an exception to the general order-independence of the keyword format. 7. VALUE is scaled in the same manner as in *DEFINE_CURVE, i.e., Scaled value = SFA×(Defined value + OFFA). 8. Unless stated otherwise in the description of a keyword command that references a table, there is no extrapolation beyond the range of VALUEs de- fined for the table. For example, if the table VALUE represents strain rate and the calculated strain rate exceeds the last/highest VALUE given by the table, the stress-strain curve corresponding to the last/highest table VALUE will be used. *DEFINE_TABLE_2D Purpose: Define a table. Unlike the *DEFINE_TABLE keyword above, a curve ID is specified for each value defined in the table. This allows the same curve ID to be referenced by multiple tables, and the curves may be defined anywhere in the input file. Other than these differences from *DEFINE_TABLE, the general rules given in the remarks of *DEFINE_TABLE still apply. Card 1 1 2 3 4 5 6 7 8 Variable TBID SFA OFFA Type I F Default none 1. F 0. Points Cards. Place one point per card. The values must be in ascending order. Input is terminated when a “*DEFINE_CURVE” keyword card is found. Card 2 1 2 3 4 Variable VALUE CURVE ID Type F I Default 0.0 none VARIABLE TBID DESCRIPTION Table ID. Tables and Load curves may not share common ID's. LS-DYNA allows load curve ID's and table ID's to be used interchangeably. SFA Scale factor for VALUE. OFFA Offset for VALUE, see explanation below. VALUE Load curve will be defined corresponding to this value. The value could be, for example, a strain rate. CURVEID Load curve ID. See Remark 1. *DEFINE 1. Though generally of no concern to the user, curve CURVEID is automatically duplicated during initialization and the duplicate curve is automatically as- signed a unique curve ID. The generated curve IDs used by the table are re- vealed in d3hsp. It is generally only necessary to know the generated curve IDs when interpreting warning messages about those curves. *DEFINE_TABLE_3D Purpose: Define a three dimensional table. For each value defined below, a table ID is specified. For example, in a thermally dependent material model, the value given below could correspond to temperature for a table ID defining effective stress versus strain curves for a set of strain rate values. Each table ID can be referenced by multiple three dimensional tables, and the tables may be defined anywhere in the input. Card 1 1 2 3 4 5 6 7 8 Variable TBID SFA OFFA Type I F Default none 1. F 0. Points Cards. Place one point per card. The values must be in ascending order. Input is terminated when a “*DEFINE_CURVE” keyword card is found. Card 2 1 2 3 4 Variable VALUE TABLE ID Type F I Default 0.0 none VARIABLE TBID DESCRIPTION Table ID. Tables and Load curves may not share common ID's. LS-DYNA allows load curve ID's and table ID's to be used interchangeably. SFA Scale factor for VALUE. OFFA Offset for VALUE, see explanation below. VALUE Load curve will be defined corresponding to this value, e.g., this value could be a strain rate for example. TABLEID Table ID. *DEFINE 1. VALUE is scaled in the same manner as in *DEFINE_CURVE, i.e., Scaled value = SFA × (Defined value + OFFA). 2. Unless stated otherwise in the description of a keyword command that references a table, there is no extrapolation beyond the range of VALUEs de- fined for the table. For example, if the table VALUE represents strain rate and the calculated strain rate exceeds the last/highest VALUE given by the table, the stress-strain curve corresponding to the last/highest table VALUE will be used *DEFINE_TABLE_MATRIX This is an alternative input format for *DEFINE_TABLE that allows for reading data from an unformatted text file containing a matrix with data separated by comma delimiters. The purpose is to use data saved directly from excel sheets without having to convert it to keyword syntax. Card 1 1 2 3 4 5 6 7 8 Variable TBID Type I FILENAME A70 Card 2 1 2 3 4 5 6 7 8 Variable NROW NCOL SROW SCOL SVAL OROW OCOL OVAL Type I I F Default None None 1. F 1. F 1. F 0. F 0. F 0. VARIABLE TBID DESCRIPTION Table ID. Tables and Load curves may not share common ID's. LS-DYNA allows load curve ID's and table ID's to be used interchangeably. FILENAME Name of file containing table data (stored as a matrix). NROW Number of rows in the matrix, same as number of rows in the file the FILENAME. interpretation of rows and columns in the read matrix, see remarks. A negative value of NROW switches NCOL Number of columns in the matrix, same as number of data entries per row in the file FILENAME SROW Scale factor for row data, see remarks. SCOL SVAL 15-268 (DEFINE) Scale factor for column data, see remarks. VARIABLE DESCRIPTION OROW Offset for row data, see remarks. Offset for column data, see remarks. Offset for matrix values, see remarks. OCOL OVAL Remarks: The use of this keyword allows for inputting a table in form of a matrix from a file, exemplified here by a 4 × 5 matrix. C1 V11 V21 V31 ⋮ C2 V12 V22 V32 ⋮ C3 V13 V23 V33 ⋮ C4 V14 V24 V34 ⋮ R1 R2 R3 ⋮ The unformatted file representing this matrix would contain the following data ,C1,C2,C3,C4 R1,V11,V12,V13,V14 R2,V21,V22,V23,V24 R3,V31,V32,V33,V34 Note that the first entry in the matrix is a dummy and delimited by an initial comma in the file. The keyword card for this matrix is: (TBID = 1000 and the filename is file.txt) *DEFINE_TABLE_MATRIX 1000,file.txt 4,5 This is equivalent to using: *DEFINE_TABLE 1000 C1 C2 C3 C4 *DEFINE_CURVE 1001 R1,V11 R2,V21 R3,V31 *DEFINE_CURVE 1002 R1,V12 R2,V22 R3,V32 *DEFINE_CURVE 1003 R1,V13 R2,V23 R3,V33 *DEFINE_CURVE 1004 R1,V14 R2,V24 R3,V34 All entries in the matrix can be scaled and offset following the convention for other tables and curves: Scaled Value = S[ROW/COL] × (Value + O[ROW/COL]) Finally, the matrix can be transposed by setting NROW to a negative value. In the example above this would mean that *DEFINE_TABLE_MATRIX 1000,file.txt -4,5 is equivalent to using: *DEFINE_TABLE 1000 R1 R2 R3 *DEFINE_CURVE 1001 C1,V11 C2,V12 C3,V13 C4,V14 *DEFINE_CURVE 1002 C1,V21 C2,V22 C3,V23 C4,V24 *DEFINE_CURVE 1003 C1,V31 C2,V32 C3,V33 C4,V34 In this case, any scaling applies to the matrix entries before transposing the data, i.e., for row entries the scaled value is and for column entries Scaled Value = SROW × (𝑅 + OROW), Scaled Value = SCOL × (𝐶 + OCOL) regardless the sign of TBID. *DEFINE_TARGET_BOUNDARY Purpose: This keyword is used to define the desired boundary of a formed part. This boundary provides the criteria used during blank-size development. The definitions associated with this keyword are used, exclusively, by the *INTERFACE_BLANKSIZE_- DEVELOPMENT feature. Point Cards. Include one card for each point in the curve. These points are interpolated to form a closed curve. This input is terminated with *END. Card 1 1 2 3 4 5 6 7 8 9 10 Variable X Y Z Type E16.0 E16.0 E16.0 Default none none none VARIABLE DESCRIPTION X, Y, Z Location coordinates of a target node. Remarks: 1. The keyword file specified on the second data card for the *INTERFACE_- BLANKSIZE_DEVELOPMENT keyword must contain a *DEFINE_TARGET_- BOUNDARY keyword. 2. A partial keyword input is shown below. Note that the input is in a 3E16.0 FORTRAN format. Also note that the first and last curve points coincide. *KEYWORD *DEFINE_TARGET_BOUNDARY -1.83355e+02 -5.94068e+02 -1.58639e+02 -1.80736e+02 -5.94071e+02 -1.58196e+02 -1.78126e+02 -5.94098e+02 -1.57813e+02 -1.75546e+02 -5.94096e+02 -1.57433e+02 -1.72888e+02 -5.94117e+02 -1.57026e+02 ⋮ ⋮ ⋮ -1.83355e+02 -5.94068e+02 -1.58639e+02 *END Typically, these boundary nodes obtained from the boundary curves for a final (trimmed) piece, or from a draw blank edge at a certain distance outside of the draw beads. LS-PrePost 4.1 can generate the points for this keyword from IGES data. To use IGES data select Curve → Convert→ Method (To Keyword) → Select *DEFINE_TARGET_BOUNDARY; pick the curves then select “To Key”. To output a keyword choose File → Save as → Save Keyword As, and select “Out- put Version” as “V971_R7”. 3. This feature is available in LS-DYNA R6 Revision 74560 and later releases. *DEFINE_TRACER_PARTICLES_2D Purpose: Define tracer particles that follow the deformation of a material. This is useful for visualizing the deformation of a part that is being adapted in a metal forming operation. Nodes used as tracer particles should only be used for visualization and not associated with anything in the model that may alter the response of the model, e.g., they should not be used in any elements except those with null materials. Card 1 1 2 3 4 5 6 7 8 Variable NSET PSET Type I Default none I 0 VARIABLE DESCRIPTION NSET PSET The node set ID for the nodes used as tracer particles. Optional part set ID. If this part set is specified, only tracer particles in these parts are updated and the others are stationary. If this part set is not specified, all tracer particles are updated. *DEFINE Purpose: Define a transformation for the INCLUDE_TRANSFORM keyword option. The *DEFINE_TRANSFORMATION command must be defined before the *IN- CLUDE_TRANSFORM command can be used. Card 1 1 2 3 4 5 6 7 8 Variable TRANID Type I Default none Transformation Cards. Include as many cards as necessary. This input ends at the next keyword (“*”) card. Card 2 1 Variable OPTION Type A 2 A1 F 3 A2 F 4 A3 F 5 A4 F 6 A5 F 7 A6 F 8 A7 F VARIABLE DESCRIPTION TRANID Transform ID. OPTION For the available options see the table below. A1-A7 Parameters. See Table 15-47 below for the available options. OPTION PARAMETERS FUNCTION MIRROR a1, a2, a3, a4, a5, a6, a7 Reflect, about a mirror plane defined to its contain normal pointing (a1, a2, a3) toward (a4, a5, a6). Setting a7 = 1 reflects the coordinate system as well, i.e., the mirrored coordinate system uses the left-hand-rule to determine the local 𝑧-axis. (a1, a2, a3) having from point the point SCALE a1, a2, a3 Scale the global x, y, and z coordinates of a point by a1, a2, and a3, respectively. If zero, a default of unity is set. ROTATE a1, a2, a3, a4, a5, a6, a7 Rotate through an angle (deg), a7, about a line with direction cosines a1, a2, and a3 passing through the point with coordinates a4, a5, and a6. TRANSL a1, a2, a3 POINT a1,a2,a3,a4 POS6P a1, a2, a3, a4, a5, a6 POS6N a1, a2, a3, a4, a5, a6 If a4 through a7 are zero, then a1 and a2 are the ID’s of two POINTs and a3 defines the rotation angle. The axis of rotation is defined by a vector going from point with ID a1 to point with ID a2. Translate the x, y, and z coordinates of a point by a1, a2, and a3, respectively. Define a point with ID, a1, with the initial coordinates a2, a3, and a4. Positioning by 6 points. Affine transfor- mation (rotation and translation, no scaling) given by three start points a1, a2, and a3 and three target points a4, a5, and a6. The six POINTs must be defined before they are referenced. Only 1 POS6P option is permitted within *DEFINE_TRANSFORMATION a definition. Positioning by 6 nodes. Affine transformation (rotation and translation, no scaling) given by three start nodes a1, a2, and a3 and three target nodes a4, a5, and a6. The six nodes must be defined before they are referenced. Only 1 POS6N option is permitted within a OPTION PARAMETERS FUNCTION *DEFINE_TRANSFORMATION definition. Table 15-47. List of allowed transformations. Each option represents a transformation matrix. When more than one option is used, the transformation matrix defined by MIRROR, SCALE, ROTATE or TRANSL is applied to the previously defined existing matrix to form the new global transformation matrix. Therefore the ordering of the SCALE, ROTATE, and TRANSL commands is important. It is generally recommended to first scale, then rotate, and finally translate the model. POS6P and POS6N differ from other options by not applying their transformation matrix to the existing global matrix. Instead the transformation matrix defined by POS6P or POS6N replaces the existing matrix and becomes the new global transformation matrix. The POINT option in ROTATE provides a means of defining rotations about axes defined by the previous transformations. The coordinates of the two POINTs are transformed by all the transformations up to the transformation where they are referenced. The POINTs must be defined before they are referenced, and their identification numbers are local to each *DEFINE_TRANSFORMATION. The coordinates of a POINT are transformed using all the transformations before it is referenced, not just the transformations between its definition and its reference. To put it another way, while the ordering of the transformations is important, the ordering between the POINTs and the transformations is not important. NOTE: When *DEFINE_TRANSFORMATION is called from within the target of an *INCLUDE_TRANS- FORM keyword, the result will involve stacked transformations. In the following example, the *DEFINE_TRANSFORMATION command is used 3 times to input the same dummy model and position it as follows: 4. Transformation id 1000 imports the dummy model (dummy.k) and rotates it 45 degrees about 𝑧-axis at the point (0.0,0.0,0.0). Transformation id 1001 performs the same transformation using the POINT option. 5. Transformation id 2000 imports the same dummy model (dummy.k) and translates 1000 units in the 𝑥 direction. 6. Transformation id 3000 imports the same dummy model (dummy.k) and translates 2000 units in the x direction. For each *DEFINE_TRANSFORMA- TION, the commands TRANSL, SCALE, and ROTATE are available. The trans- formations are applied in the order in which they are defined in the file, e.g., transformation id 1000 in this example would translate, scale and then rotate the model. *INCLUDE_TRANSFORM uses a transformation id defined by a *DEFINE_TRANSFORMATION command to import a model and perform the associated transformations. It also allows the user upon importing the model to apply offsets to the various entity ids and perform unit conversion of the im- ported model. *KEYWORD *DEFINE_TRANSFORMATION 1000 $ option & dx& dy& dz& TRANSL 0000.0 0.0 0.0 $ option & dx& dy& dz& SCALE 1.00 1.0 1.0 $ option & dx& dy& dz& px& py& pz& angle& ROTATE 0.00 0.0 1.0 0.00 0.00 0.0 45.00 *DEFINE_TRANSFORMATION 1001 POINT 1 0.0 0.0 0.0 POINT 2 0.0 0.0 1.0 ROTATE 1 2 45.0 *DEFINE_TRANSFORMATION 2000 $ option & dx& dy& dz& TRANSL 1000.0 0.0 0.0 *DEFINE_TRANSFORMATION $ tranid & 3000 $ option & dx& dy& dz& TRANSL 2000.0 0.0 0.0 *INCLUDE_TRANSFORM dummy.k $idnoff & ideoff& idpoff& idmoff & idsoff & iddoff& iddoff & 0 0 0 0 0 0 0 $ idroff& ilctmf& 0 0 $ fctmas& fcttim& fctlen& fcttem & incout& 1.0000 1.0000 1.00 1.0 1 $ tranid & 1000 *INCLUDE_TRANSFORM dummy.k $idnoff & ideoff& idpoff& idmoff & idsoff & iddoff& iddoff & 1000000 1000000 1000000 1000000 1000000 1000000 1000000 $ idroff& ilctmf& 1000000 1000000 $ fctmas& fcttim& fctlen& fcttem & incout& 1.0000 1.0000 1.00 1.0 1 $ tranid & 2000 *INCLUDE_TRANSFORM dummy.k $idnoff & ideoff& idpoff& idmoff & idsoff & iddoff& iddoff & 2000000 2000000 2000000 2000000 2000000 2000000 2000000 $ idroff& ilctmf& 2000000 2000000 $ fctmas& fcttim& fctlen& fcttem & incout& 1.0000 1.0000 1.00 1.0 1 $ tranid & 3000 *END *DEFINE_TRIM_SEED_POINT_COORDINATES Purpose: The keyword is developed to facilitate blank trimming in a stamping line die simulation. It allows for the trimming process and inputs to be defined independent of the previous process simulation results, and is applicable to shell, solid and laminate. Card 1 1 Variable NSEED Type I Default none 2 X1 F 0 3 Y1 F 0 4 Z1 F 0 5 X2 F 0 6 Y2 F 7 Z2 F 0.0 0.0 8 VARIABLE DESCRIPTION NSEED Number of seed points. Maximum value of “2” is allowed. X1, Y1, Z1 Location coordinates of seed point #1. X2, Y2, Z2 Location coordinates of seed point #2. Remarks: 1. This keyword is used in conjunction with keywords *ELEMENT_TRIM and *DEFINE_CURVE_TRIM, where variables NSEED1 and NSEED2 should be left as blank. For detailed usage, refer to Seed Node Definition section in *DE- FINE_CURVE_TRIM. 2. Variable NSEED is set to the number of seed points desired. For example, in a double attached drawn panel trimming, NSEED would equal to 2. 3. A partial keyword inputs for a single drawn panel trimming is listed below. *INCLUDE_TRIM drawn.dynain *ELEMENT_TRIM 1 *DEFINE_CURVE_TRIM_NEW $# TCID TCTYPE TFLG TDIR TCTOL TOLN NSEED 1 2 11 0.250 trimlines.iges *DEFINE_TRIM_SEED_POINT_COORDINATES $ NSEED X1 Y1 Z1 X2 Y2 Z2 1 -271.4 89.13 1125.679 *DEFINE_VECTOR 11,0.0,0.0,0.0,0.0,0.0,10.0 Typically, seed point coordinates can be selected from the stationary post in punch home position. 4. This feature is available in LS-DYNA R4 Revision 53048 and later releases. *DEFINE_VECTOR Purpose: Define a vector by defining the coordinates of two points. Card 1 Variable VID Type Default I 0 Remarks 2 XT F 3 YT F 4 ZT F 5 XH F 6 YH F 7 ZH F 0.0 0.0 0.0 0.0 0.0 0.0 8 CID I 0 VARIABLE DESCRIPTION VID Vector ID X-coordinate of tail of vector Y-coordinate of tail of vector Z-coordinate of tail of vector X-coordinate of head of vector Y-coordinate of head of vector Z-coordinate of head of vector Coordinate system ID to define vector in local coordinate system. All coordinates, XT, YT, ZT, XH, YH, and ZH are in respect to CID. EQ.0: global (default). XT YT ZT XH YH ZH CID Remarks: 1.The coordinates should differ by a certain margin to avoid numerical inaccuracies. Purpose: Define a vector with two nodal points. *DEFINE Card 1 2 3 4 5 6 7 8 Variable VID NODET NODEH Type Default I 0 I 0 I 0 VARIABLE DESCRIPTION VID Vector ID NODET Nodal point to define tail of vector NODEH Nodal point to define head of vector EXAMPLES The following examples demonstrate the input for these options: *DEFINE_BOX *DEFINE_COORDINATE_NODES, *DEFINE_COORDINATE_SYSTEM, *DEFINE_COORDINATE_VECTOR *DEFINE_CURVE *DEFINE_SD_ORIENTATION *DEFINE_VECTOR commands. $$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ $ $$$$ *DEFINE_BOX $ $$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ $ $ Define box number eight which encloses a volume defined by two corner $ points: (-20.0, -39.0, 0.0) and (20.0, 39.0, 51.0). As an example, this $ box can be used as an input for the *INITIAL_VELOCITY keyword in which $ all nodes within this box are given a specific initial velocity. $ *DEFINE_BOX $ $...>....1....>....2....>....3....>....4....>....5....>....6....>....7....>....8 $ boxid xmm xmx ymn ymx zmn zmx 8 -20.0 20.0 -39.0 39.0 0.0 51.0 $ $$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ $$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ $ $$$$ *DEFINE_COORDINATE_NODES $ $$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ $ $ Define local coordinate system number 5 using three nodes: 10, 11 and 20. $ Nodes 10 and 11 define the local x-direction. Nodes 10 and 20 define $ the local x-y plane. $ $ For example, this coordinate system (or any coordinate system defined using $ a *DEFINE_COORDINATE_option keyword) can be used to define the local $ coordinate system of a joint, which is required in order to define joint $ stiffness using the *CONSTRAINED_JOINT_STIFFNESS_GENERALIZED keyword. $ *DEFINE_COORDINATE_NODES $ $...>....1....>....2....>....3....>....4....>....5....>....6....>....7....>....8 $ cid n1 n2 n3 5 10 11 20 $ $$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ $$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ $ $$$$ *DEFINE_COORDINATE_SYSTEM $ $$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ $ $ Define local coordinate system number 3 using three points. The origin of $ local coordinate system is at (35.0, 0.0, 0.0). The x-direction is defined $ from the local origin to (35.0, 5.0, 0.0). The x-y plane is defined using $ the vector from the local origin to (20.0, 0.0, 20.0) along with the local $ x-direction definition. $ *DEFINE_COORDINATE_SYSTEM $ $...>....1....>....2....>....3....>....4....>....5....>....6....>....7....>....8 $ cid Xo Yo Zo Xl Yl Zl 3 35.0 0.0 0.0 35.0 5.0 0.0 $ $ Xp Yp Zp 20.0 0.0 20.0 $ $$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ $$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ $ $$$$ *DEFINE_COORDINATE_VECTOR $ $$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ $ $ Define local coordinate system number 4 using two vectors. $ Vector 1 is defined from (0.0, 0.0, 0.0) to (1.0, 1.0, 0.0) $ Vector 2 is defined from (0.0, 0.0, 0.0) to (1.0, 1.0, 1.0) $ See the corresponding keyword command for a description. $ *DEFINE_COORDINATE_VECTOR $ $...>....1....>....2....>....3....>....4....>....5....>....6....>....7....>....8 $ cid Xx Yx Zx Xv Yv Zv 4 1.0 1.0 0.0 1.0 1.0 1.0 $ $$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ $$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ $ $$$$ *DEFINE_CURVE $ $$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ $ $ Define curve number 517. This particular curve is used to define the $ force-deflection properties of a spring defined by a *MAT_SPRING_INELASTIC $ keyword. The abscissa value is offset 25.0 as a means of modeling a gap $ at the front of the spring. This type of spring would be a compression $ only spring. $ *DEFINE_CURVE $ $...>....1....>....2....>....3....>....4....>....5....>....6....>....7....>....8 $ lcid sidr scla sclo offa offo 517 25.0 $ $ abscissa ordinate 0.0 0.0 80.0 58.0 95.0 35.0 150.0 44.5 350.0 45.5 $ $$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ $$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ $ $$$$ *DEFINE_SD_ORIENTATION $ $$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ $ $ A discrete spring is defined with two nodes in 3-D space. However, it is $ desired to have the force of that spring to act only in the z-direction. $ The following definition makes this happen. Additionally, vid = 7 $ must be specified in the *ELEMENT_DISCRETE keyword for this spring. $ *DEFINE_SD_ORIENTATION $ $...>....1....>....2....>....3....>....4....>....5....>....6....>....7....>....8 $ vid iop xt yt zt nid1 nid2 7 0 0.0 0.0 1.0 $ $$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ $$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ $ $$$$ *DEFINE_VECTOR $ $$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ $ $ Define vector number 5 from (0,0,0) to (0,1,1). As an example, this vector $ can be used to define the direction of the prescribed velocity of a node $ using the *BOUNDARY_PRESCRIBED_MOTION_NODE keyword. $ *DEFINE_VECTOR $ $...>....1....>....2....>....3....>....4....>....5....>....6....>....7....>....8 $ vid xt yt zt xh yh zh 3 0.0 0.0 0.0 0.0 1.0 1.0 $ $$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ The cards in this section are defined in alphabetical order and are as follows: *DEFORMABLE_TO_RIGID *DEFORMABLE_TO_RIGID_AUTOMATIC *DEFORMABLE_TO_RIGID_INERTIA If one of these cards is defined, then any deformable part defined in the model may be switched to rigid during the calculation. Parts that are defined as rigid (*MAT_RIGID) in the input are permanently rigid and cannot be changed to deformable. Deformable parts may be switched to rigid at the start of the calculation by specifying them on the *DEFORMABLE_TO_RIGID card. Part switching may be specified on a restart or it may be performed automatically by use of the *DEFORMABLE_TO_RIGID_AUTO- MATIC cards. The *DEFORMABLE_TO_RIGID_INERTIA cards allow inertial properties to be defined for deformable parts that are to be swapped to rigid at a later stage. It is not possible to perform part material switching on a restart if it was not flagged in the initial analysis. The reason for this is that extra memory needs to be set up internally to allow the switching to take place. If part switching is to take place on a restart, but no parts are to be switched at the start of the calculation, no inertia properties for switching and no automatic switching sets are to be defined, then just define one *DEFORMABLE_TO_RIGID card without further input. *DEFORMABLE_TO_RIGID Purpose: Define materials to be switched to rigid at the start of the calculation. Card 1 2 3 4 5 6 7 8 Variable PID MRB PTYPE Type I Default none A I 0 VARIABLE DESCRIPTION PID MRB Part ID of the part which is switched to a rigid material, also see *PART. Part ID of the master rigid body to which the part is merged. If zero, the part becomes either an independent or master rigid body. PTYPE Type of PID: EQ.“PART”: PID is a part ID. EQ.“PSET”: PID is a part set ID. All parts included in part set PID will be switched to rigid at the start of the cal- culation. *DEFORMABLE_TO_RIGID_AUTOMATIC Purpose: Define a set of parts to be switched to rigid or to deformable at some stage in the calculation This keyword’s data cards are enumerated below: • 2 parameter cards: see “Card 1” and “Card 2” below • D2R instances of “Card 3” • R2D instances of “Card 4” • Total number of cards = 2 + D2R + R2D Card 1 1 2 3 4 5 6 7 8 Variable SWSET CODE TIME 1 TIME 2 TIME 3 ENTNO RELSW PAIRED Type I Default none Remark Card 2 1 I 0 1 2 F 0. F 1020 F 0. I 0 I 0. 1, 2 3 4 5 6 7 I 0 3 8 Variable NRBF NCSF RWF DTMAX D2R R2D OFFSET Type Default I 0 I 0 I 0 F 0. I 0 I 0 F 0 VARIABLE DESCRIPTION SWSET Set number for this automatic switch set. Must be unique. CODE Activation switch code. Defines the test to activate the automatic material switch of the part: EQ.0: switch takes place at time 1, EQ.1: switch takes place between time 1 and time 2 if rigid wall force (specified below) is zero, EQ.2: switch takes place between time 1 and time 2 if contact VARIABLE DESCRIPTION surface force (specified below) is zero, EQ.3: switch takes place between time 1 and time 2 if rigid wall force (specified below) is non-zero, EQ.4: switch takes place between time 1 and time 2 if contact surface force (specified below) is non-zero. EQ.5: switch is controlled by *SENSOR_CONTROL with When column 8, TYPE = DEF2RIG, see *SENSOR_CONTROL. CODE = 5, TIME1~PAIRED, are ignored. column 3 inputs of to TIME1 TIME2 TIME3 Switch will not take place before this time. Switch will not take place after this time: EQ.0: Time 2 set to 1020 Delay period. After this part switch has taken place, another automatic switch will not take place for the duration of the delay period. If set to zero a part switch may take place immediately after this switch. ENTNO Rigid wall/contact surface number for switch codes 1, 2, 3, 4. RELSW Related switch set. The related switch set is another automatic switch set that must be activated before this part switch can take place: EQ.0: no related switch set. PAIRED Define a pair of related switches. EQ.0: not paired EQ.1: paired with switch set RELSW and is the Master switch. EQ.-1: paired with switch set RELSW and is the Slave switch. VARIABLE NRBF DESCRIPTION Nodal rigid body flag. For all values of NRBF, nodal rigid bodies defined using *CON- STRAINED_NODAL_RIGID_BODY and *CONSTRAINED_GEN- ERALIZED_WELD_OPTION, which share any nodes with a rigid body created by deformable-to-rigid switching, are merged with the latter to form a single rigid body. Other actions dependent upon the value of NRBF are: EQ.0: no further action, EQ.1: delete all remaining nodal rigid bodies, that is, delete those nodal rigid bodies that do not share any nodes with a rigid body created by deformable-to-rigid switch- ing, EQ.2: Activate nodal rigid bodies. NCSF Nodal constraint set flag. If nodal constraint/spot weld definitions are active in the deformable bodies that are switched to rigid, then the definitions should be deleted to avoid instabilities: EQ.0: no change, EQ.1: delete, EQ.2: activate. RWF Flag to delete or activate rigid walls: EQ.0: no change, EQ.1: delete, EQ.2: activate. DTMAX Maximum permitted time step size after switch. D2R Number of deformable parts to be switched to rigid plus number of rigid parts for which new master/slave rigid body combinations will be defined: EQ.0: no parts defined. R2D Number of rigid parts to be switched to deformable: EQ.0: no parts defined. VARIABLE OFFSET DESCRIPTION Optional contact thickness for switch to deformable. For contact, its value should be set to a value greater than the contact thickness offsets to ensure the switching occurs prior to impact. This option applies if and only if CODE is set to 3 or 4. For CODE = 3 all rigid wall options are implemented. For CODE = 4, the implementation works for the contact type CONTACT_AU- TOMATIC_when the options: ONE_WAY_SURFACE_TO_SUR- FACE, NODES_TO_SURFACE, and SUR-FACE_TO_SURFACE are invoked. Deformable to Rigid Cards. D2R additional cards with one for each part. Card 3 1 2 3 4 5 6 7 8 Variable PID MRB PTYPE Type I Default none A I 0 VARIABLE DESCRIPTION PID MRB Part ID of the part which is switched to a rigid material. When PID is merged to another rigid body by the MRB field, this part is allowed to be rigid before the switch. Part ID of the master rigid body to which part PID is merged. If zero, part PID becomes either an independent or master rigid body. PTYPE Type of PID: EQ.“PART”: PID is a part ID. EQ.“PSET”: PID is a part set ID. Rigid to Deformable Cards. R2D additional cards with one for each part. Card 4 1 2 3 4 5 6 7 8 Variable PID PTYPE Type I A Default none VARIABLE DESCRIPTION PID Part ID of the part which is switched to a deformable material. PTYPE Type of PID: EQ.“PART”: PID is a part ID. EQ.“PSET”: PID is a part set ID. Remarks: 1. Allowed Contact Types. Only surface to surface and node to surface contacts can be used to activate an automatic part switch. 2. Rigid Wall Numbering. Rigid wall numbers are the order in which they are defined in the deck. The first rigid wall and the first contact surface encoun- tered in the input deck will have an entity number of 1. The contact surface id is that as defined on the *CONTACT_…_ID card. 3. Paired Switches. Switch sets may be paired together to allow a pair of switches to be activated more than once. Each pair of switches should use consistent values for CODE, i.e. 1 & 3 or 2 & 4. Within each pair of switches, the related switch, RELSW, should be set to the ID of the other switch in the pair. The Master switch (PAIRED = 1) will be activated before the Slave switch (PAIRED = -1). Pairing allows the multiple switches to take place as for exam- ple when contact is made and lost several times during an analysis. If the delete switch is activated, ALL corresponding constraints are deactivated regardless of their relationship to a switched part. By default, constraints which are directly associated with a switched part are deactivated/activated as neces- sary. $ Define a pair or related switches that will be activated by (no)force on $ Contact 3. To start with switch set 20 will be activated (PAIRED=1) swapping $ the PARTS to RIGID. When the contact force is none zero switch set 10 will be $ activated swapping the PARTS to DEFORMABLE. If the contact force returns to $ zero switch set 20 will be activated again making the PARTS RIGID. $ *DEFORMABLE_TO_RIGID_AUTOMATIC $...>....1....>....2....>....3....>....4....>....5....>....6....>....7....>... .8 $ swset code time 1 time 2 time 3 entno relsw paired 20 2 3 10 1 $ nrbf ncsf rwf dtmax D2R R2D 1 *DEFORMABLE_TO_RIGID_AUTOMATIC $...>....1....>....2....>....3....>....4....>....5....>....6....>....7....>... .8 $ swset code time 1 time 2 time 3 entno relsw paired 10 4 3 20 -1 $ nrbf ncsf rwf dtmax D2R R2D 1 *DEFORMABLE_TO_RIGID_INERTIA Purpose: Inertial properties can be defined for the new rigid bodies that are created when the deformable parts are switched. These can only be defined in the initial input if they are needed in a later restart. Unless these properties are defined, LS-DYNA will recompute the new rigid body properties from the finite element mesh. The latter requires an accurate mesh description. When rigid bodies are merged to a master rigid body, the inertial properties defined for the master rigid body apply to all members of the merged set. Card 1 1 2 3 4 5 6 7 8 Variable PID Type I Default none Card 2 Variable 1 XC Type F Card 3 1 Variable IXX 2 YC F 2 IXY 3 ZC F 3 IXZ 4 TM F 4 IYY 5 6 7 8 5 IYZ 6 IZZ 7 8 Type F F F F F F Default none 0.0 0.0 none 0.0 none VARIABLE DESCRIPTION PID XC YC Part ID, see *PART. x-coordinate of center of mass y-coordinate of center of mass VARIABLE DESCRIPTION ZC TM IXX IXY IXZ IYY IYZ IZZ z-coordinate of center of mass Translational mass Ixx (the xx component of inertia tensor) Ixy Ixz Iyy Iyz Izz The element cards in this section are defined in alphabetical order: *ELEMENT_BLANKING *ELEMENT_BEAM_{OPTION}_{OPTION} *ELEMENT_BEAM_PULLEY *ELEMENT_BEAM_SOURCE *ELEMENT_DIRECT_MATRIX_INPUT *ELEMENT_DISCRETE_{OPTION} *ELEMENT_DISCRETE_SPHERE_{OPTION} *ELEMENT_GENERALIZED_SHELL *ELEMENT_GENERALIZED_SOLID *ELEMENT_INERTIA_{OPTION} *ELEMENT_INTERPOLATION_SHELL *ELEMENT_INTERPOLATION_SOLID *ELEMENT_LANCING *ELEMENT_MASS_{OPTION} *ELEMENT_MASS_MATRIX_{OPTION} *ELEMENT_MASS_PART_{OPTION} *ELEMENT_PLOTEL *ELEMENT_SEATBELT *ELEMENT_SEATBELT_ACCELEROMETER *ELEMENT_SEATBELT_PRETENSIONER *ELEMENT_SEATBELT_RETRACTOR *ELEMENT_SEATBELT_SENSOR *ELEMENT_SHELL_{OPTION} *ELEMENT_SHELL_NURBS_PATCH *ELEMENT_SHELL_SOURCE_SINK *ELEMENT_SOLID_{OPTION} *ELEMENT_SOLID_NURBS_PATCH *ELEMENT_SPH *ELEMENT_TRIM *ELEMENT_TSHELL_{OPTION} The ordering of the element cards in the input file is completely arbitrary. An arbitrary number of element blocks can be defined preceded by a keyword control card. *ELEMENT Purpose: This keyword is used to define a part set to be used in keyword *DEFINE_- FORMING_BLANKMESH for a blank mesh generation. Card 1 1 2 3 4 5 6 7 8 Variable PSID Type I Default none VARIABLE DESCRIPTION PSID Part set ID, defined by *SET_PART. Remarks: 1. This keyword is used in conjunction with *DEFINE_FORMING_BLANKMESH to generate mesh on a sheet blank for metal forming simulation. 2. This feature is available in LS-DYNA R5 Revision 59165 or later releases. *ELEMENT_BEAM_{OPTION}_{OPTION} Available options include: <BLANK> THICKNESS, SCALAR, SCALR or SECTION PID OFFSET ORIENTATION WARPAGE ELBOW (beta) Purpose: Define two node elements including 3D beams, trusses, 2D axisymmetric shells, and 2D plane strain beam elements. The type of the element and its formulation is specified through the part ID and the section ID . Two alternative methods are available for defining the cross sectional property data. The THICKNESS and SECTION options are provided for the user to override the *SEC- TION_BEAM data which is taken as the default if the THICKNESS or SECTION option is not used. . The SECTION option applies only to resultant beams (ELFORM.eq.2 on *SECTION_BEAM). End release conditions are imposed using constraint equations, and caution must be used with this option as discussed in remark 2 below. The SCALAR/SCALR options applies only to material model type 146, *MAT_1DOF_GEN- ERALIZED_SPRING. The PID option is used by the type 9 spot weld element only and is ignored for all other beam types. When the PID option is active an additional card is read that gives two part ID's that are tied by the spot weld element. If the PID option is inactive for the type 9 element the nodal points of the spot weld are located to the two nearest master segments. In either case, *CONTACT_SPOTWELD must be defined with the spot weld beam part as slave and the shell parts (including parts PID1 and PID2) as master. The surface of each segment should project to the other and in the most typical case the node defining the weld, assuming only one node is used, should lie in the middle; however, this is not a requirement. Note that with the spot weld elements only one node is needed to define the weld, and two nodes are optional. The options ORIENTATION and OFFSET are not available for discrete beam elements. The ELBOW option is a 3-node beam element with quadratic interpolation that is tailored for the piping industry. It includes 12 degrees of freedom, including 6 ovalization degrees of freedom for describing the ovalization, per node. That is a total of 36 DOFs for each element. An internal pressure can also be given that tries to stiffen the pipe. The pressure, if activated accordingly, can also contribute to the elongation of the pipe. The control node must be given but it is only used for initially straight elbow elements. For curved elements the curvature center is used as the control node. See *SECTION_BEAM for more information about the physical properties such as pressure and output options. Card 1 1 2 3 4 5 6 7 8 9 10 Variable EID PID N1 N2 N3 RT1 RR1 RT2 RR2 LOCAL Type I I I I I I Default none none none none none 0 I 0 I 0 I 0 I 2 Remarks 1 2,3 2,3 2,3 2,3 2,3 Thickness Card. Additional Card for THICKNESS keyword option. Card 1 2 3 4 5 6 7 8 9 10 Variable PARM1 PARM2 PARM3 PARM4 PARM5 Type Remarks F 5 F 5 F 5 F 5 Section Card. Additional card required for SECTION keyword option. Card 1 Variable STYPE Type A 2 D1 F 3 D2 F 4 D3 F 5 D4 F 6 D5 F 7 D6 F F 5,6 8 Remarks Scalar card. Additional card for SCALAR keyword option. Card 1 2 3 4 5 6 7 8 9 10 Variable VOL INER Type F F CID F DOFN1 DOFN2 F F Scalar Card (alternative). Additional card for SCALR keyword option. Card 1 2 3 4 5 6 7 8 9 10 Variable VOL INER CID1 CID2 DOFNS Type F F F F F Spot Weld Part Card. Additional card for PID keyword option. Card 1 2 3 4 5 6 7 8 9 10 Variable PID1 PID2 Type I I Default none none Remarks Offset Card. Additional card for OFFSET keyword option. Card 1 2 3 4 5 6 7 8 Variable WX1 WY1 WZ1 WX2 WY2 WZ2 Type F F F F F F Default 0.0 0.0 0.0 0.0 0.0 0.0 Remarks 8 8 8 8 8 8 Orientation Card. Additional card for ORIENTATION keyword option. 4 5 6 7 8 Card Variable 1 VX Type F 2 VY F 3 VZ F Default 0.0 0.0 0.0 Remarks Warpage Card. Additional card for WARPAGE keyword option. Card 1 2 3 4 5 6 7 8 Variable SN1 SN2 Type I I Default none none Remarks Elbow Card. Additional card for ELBOW keyword option. Card 1 2 3 4 5 6 7 8 Variable MN Type I Default none Remarks VARIABLE EID PID N1 N2 N3 DESCRIPTION Element ID. A unique ID is generally required, i.e., EID must be different from the element ID’s also defined under *ELEMENT_- DISCRETE and *ELEMENT_SEATBELT. If the parameter, BEAM, is set to 1 on the keyword input for *DATABASE_BINA- RY_D3PLOT, the null beams used for visualization are not created for the latter two types, and the ID’s used for the discrete elements and the seatbelt elements can be identical to those defined here. Part ID, see *PART. Nodal point (end) 1. Nodal point (end) 2. This node is optional for the spot weld, beam type 9, since if it not defined it will be created automatically and given a non-conflicting nodal point ID. Nodes N1 and N2 are automatically positioned for the spot weld beam element. For the zero length discrete beam elements where one end is attached to ground, set N2 = -N1. In this case, a fully constrained nodal point will be created with a unique ID for node N2. Nodal point 3 for orientation. The third node, N3, is optional for beam types 3, 6, 7, 8, and if the cross-section is circular, beam types 1 and 9. The third node is used for the discrete beam, type 6, if and only if SCOOR is set to 2.0 in the *SECTION_BEAM input, but even in this case it is optional. An orientation vector can be defined directly by using the option, ORIENTATION. In this case N3 can be defined as zero. RT1, RT2 Release conditions for translations at nodes N1 and N2, VARIABLE DESCRIPTION respectively: EQ.0: no translational degrees-of-freedom are released EQ.1: x-translational degree-of-freedom EQ.2: y-translational degree-of-freedom EQ.3: z-translational degree-of-freedom EQ.4: x and y-translational degrees-of-freedom EQ.5: y and z-translational degrees-of-freedom EQ.6: z and x-translational degrees-of-freedom EQ.7: x, y, and z-translational degrees-of-freedom (3DOF) This option does not apply to the spot weld, beam type 9. RR1, RR2 Release conditions for rotations at nodes N1 and N2, respectively: EQ.0: no rotational degrees-of-freedom are released EQ.1: x-rotational degree-of-freedom EQ.2: y-rotational degree-of-freedom EQ.3: z-rotational degree-of-freedom EQ.4: x and y-rotational degrees-of-freedom EQ.5: y and z-rotational degrees-of-freedom EQ.6: z and x-rotational degrees-of-freedom EQ.7: x, y, and z-rotational degrees-of-freedom (3DOF) This option does not apply to the spot weld, beam type 9. LOCAL Coordinate system option for release conditions: EQ.1: global coordinate system EQ.2: local coordinate system (default) PARM1 Based on beam type: Type.EQ.1: beam thickness, s direction at node 1 Type.EQ.2: area Type.EQ.3: area Type.EQ.4: beam thickness, s direction at node 1 Type.EQ.5: beam thickness, s direction at node 1 VARIABLE DESCRIPTION Type.EQ.6: volume, see description for VOL below. Type.EQ.7: beam thickness, s direction at node 1 Type.EQ.8: beam thickness, s direction at node 1 Type.EQ.9: beam thickness, s direction at node 1 PARM2 Based on beam type: Type.EQ.1: beam thickness, s direction at node 2 Type.EQ.2: Iss Type.EQ.3: ramp-up time for dynamic relaxation Type.EQ.4: beam thickness, s direction at node 2 Type.EQ.5: beam thickness, s direction at node 2 Type.EQ.6: Inertia, see description for INER below. Type.EQ.7: beam thickness, s direction at node 2 Type.EQ.8: beam thickness, s direction at node 2 Type.EQ.9: beam thickness, s direction at node 2 PARM3 Based on beam type: Type.EQ.1: beam thickness, t direction at node 1 Type.EQ.2: Itt Type.EQ.3: initial stress for dynamic relaxation Type.EQ.4: beam thickness, t direction at node 1 Type.EQ.5: beam thickness, t direction at node 1 Type.EQ.6: local coordinate ID Type.EQ.7: not used. Type.EQ.8: not used. Type.EQ.9: beam thickness, t direction at node 1 PARM4 Based on beam type: Type.EQ.1: beam thickness, t direction at node 2 Type.EQ.2: Irr Type.EQ.3: not used Type.EQ.4: beam thickness, t direction at node 2 VARIABLE DESCRIPTION Type.EQ.5: beam thickness, t direction at node 2 Type.EQ.6: area Type.EQ.7: not used. Type.EQ.8: not used. Type.EQ.9: beam thickness, t direction at node 2 PARM5 Based on beam type: Type.EQ.1: not used Type.EQ.2: shear area Type.EQ.3: not used Type.EQ.4: not used Type.EQ.5: not used Type.EQ.6: offset Type.EQ.7: not used. Type.EQ.8: not used. Type.EQ.9: print flag to SWFORC file. The default is taken from the SECTION_BEAM input. To override set PARM5 to 1.0 to suppress printing, and to 2.0 to print. STYPE Section type (A format) of resultant beam, see Figure 36-1: EQ.SECTION_01: I-Shape EQ.SECTION_02: Channel EQ.SECTION_03: L-Shape EQ.SECTION_04: T-Shape EQ.SECTION_05: Tubular box EQ.SECTION_06:Z-Sape EQ.SECTION_07: Trapezoidal EQ.SECTION_08: Circular EQ.SECTION_09: Tubular EQ.SECTION_10: I-Shape 2 EQ.SECTION_11: Solid box EQ.SECTION_12: Cross EQ.SECTION_13: H-Shape EQ.SECTION_14: T-Shape 2 EQ.SECTION_15: I-Shape 3 EQ.SECTION_16: Channel 2 EQ.SECTION_17: Channel 3 EQ.SECTION_18: T-Shape 3 EQ.SECTION_19: Box-Shape 2 EQ.SECTION_20: Hexagon EQ.SECTION_21: Hat-Shape EQ.SECTION_22: Hat-Shape 2 D1-D6 Input parameters for section option using STYPE above. VARIABLE DESCRIPTION PID1 PID2 VOL INER CID DOFN1 DOFN2 CID1 CID2 Optional part ID for spot weld element type 9. Optional part ID for spot weld element type 9. Volume of discrete beam and scalar (MAT_146) beam. If the mass density of the material model for the discrete beam is set to unity, the magnitude of the lumped mass can be defined here instead. This lumped mass is partitioned to the two nodes of the beam element. The translational time step size for the type 6 beam is dependent on the volume, mass density, and the translational stiffness values, so it is important to define this parameter. Defining the volume is also essential for mass scaling if the type 6 beam controls the time step size. Mass moment of inertia for the six degree of freedom discrete beam and scalar (MAT_146) beam. This lumped inertia is partitioned to the two nodes of the beam element. The rotational time step size for the type 6 beam is dependent on the lumped inertia and the rotational stiffness values, so it is important to define this parameter if the rotational springs are active. Defining the rotational inertia is also essential for mass scaling if the type 6 beam rotational stiffness controls the time step size. Coordinate system ID for orientation, material type 146, see *DE- FINE_COORDINATE_SYSTEM. If CID = 0, a default coordinate system is defined in the global system. Active degree-of-freedom at node 1, a number between 1 to 6 where 1, 2, and 3 are the x, y, and z-translations and 4, 5, and 6 are the x, y, and z-rotations. This degree-of-freedom acts in the local system given by CID above. This input applies to material model type 146. Active degree-of-freedom at node 2, a number between 1 to 6. This degree-of-freedom acts in the local system given by CID above. This input applies to material model type 146. Coordinate system ID at node 1 for orientation, material type 146, see *DEFINE_COORDINATE_SYSTEM. If CID1 = 0, a default coordinate system is defined in the global system. Coordinate system ID at node 2 for orientation, material type 146, see *DEFINE_COORDINATE_SYSTEM. If CID2 = 0, a default coordinate system is defined in the global system. VARIABLE DOFNS DESCRIPTION Active degrees-of-freedom at node 1 and node 2. A two-digit number, the first for node 1 and the second for node 2, between 11 to 66 is expected where 1, 2, and 3 are the x, y, and z- translations and 4, 5, and 6 are the x, y, and z-rotations. These degrees-of-freedom acts in the local system given by CID1 and CID2 above. This input applies to material model type 146. If DOFNS = 12 the node one has an x-translation and node 2 has a y translation. WX1-WZ1 Offset vector at nodal point N1. See Remark 8. WX2-WZ2 Offset vector at nodal point N2. See Remark 8. VX,VY,VZ Coordinates of an orientation vector relative to node N1. In this case, the orientation vector points to a virtual third node and so the input variable N3 should be left undefined. SN1 SN2 Scalar nodal point (end) 1. This node is required for the WARPAGE option. Scalar nodal point (end) 2. This node is required for the WARPAGE option. The third node, i.e. the reference node, must be unique to each beam element if the coordinate update option is used, see *CONTROL_OUTPUT. n3 n2 n1 Figure 17-1. LS-DYNA beam elements. Node n3 determines the initial orientation of the cross section. VARIABLE DESCRIPTION MN Middle node for the ELBOW element. See Remark 9. Remarks: 1. A plane through N1, N2, and N3 defines the orientation of the principal r-s plane of the beam, see Figure 17-1. 2. This option applies to all three-dimensional beam elements. The released degrees-of-freedom can be either global, or local relative to the local beam co- ordinate system, see Figure 17-1. A local coordinate system is stored for each node of the beam element and the orientation of the local coordinate systems rotates with the node. To properly track the response, the nodal points with a released resultant are automatically replaced with new nodes to accommodate the added degrees-of-freedom. Then constraint equations are used to join the nodal points together with the proper release conditions imposed. Nodal points which belong to beam elements which have re- lease conditions applied cannot be subjected to other con- straints such as applied displacement/velocity/acceleration boundary conditions, nodal rigid bodies, nodal constraint sets, or any of the constraint type contact definitions. Force type loading conditions and penalty based contact algorithms may be used with this option. 3. Please note that this option may lead to nonphysical constraints if the translational degrees-of-freedom are released, but this should not be a problem if the displacements are infinitesimal. 4. 5. If the THICKNESS option is not used, or if THICKNESS is used but essential PARMx values are not provided, beam properties are taken from *SECTION_- BEAM. In the case of the THICKNESS option for type 6, i.e., discrete beam elements, PARM1 through PARM5 replace the first five parameters on card 2 of *SEC- TION_BEAM. Cables are a subset of type 6 beams. PARM1 is for non-cable discrete beams and is optional for cables, PARM2 and PARM3 apply only to non-cable discrete beams, and PARM4 and PARM5 apply only to cables. 6. In the THICKNESS option, PARM5 applies only to beam types 2, 6 (cables only), and 9. 7. The stress resultants are output in local coordinate system for the beam. Stress information is optional and is also output in the local system for the beam. 8. Beam offsets are sometimes necessary for correctly modeling beams that act compositely with other elements such as shells or other beams. When the OFF- SET option is specified, global X, Y, and Z components of two offset vectors are given, one vector for each of the two beam nodes. The offset vector extends from the beam node (N1 or N2) to the reference axis of the beam. The beam reference axis lies at the origin of the local s and t axes. For beam formulations 1 and 11, this origin is halfway between the outermost surfaces of the beam cross-section. Note that for cross-sections that are not doubly symmetric, e.g, a T-section, the reference axis does not pass through the centroid of the cross- section. For beam formulation 2, the origin is at the centroid of the cross- section. n1 n3 n4 n2 Figure 17-2. LS-DYNA Elbow element. Node n4 is the control node and is given as the beam center of curvature. 9. The Elbow beam is defined with 4 nodes, see Figure 17-2. Node n1, n2 being the end nodes, and node n3 is the middle node. It is custom to set n3 at the midpoint of the beam. Node n4 is an orientation node that should be at the curvature center of the beam. If a straight beam is defined initially, the orienta- tion node must be defined and should be on the convex side of the beam. If a curved beam is defined initially the orientation node is automatically calculated as the center of the beam curvature. However, an orientation node is still re- quired at the input. The extra nodes that include the ovalization degree of freedom are written to the messag file during initialization. These extra nodes have 3 dofs each. That means that there are 2 extra nodes for each physical node. For example it can look something like this: ELBOW BEAM: 1 n1-n3-n2: 1 3 2 ovalization nodes: 5 7 6 8 10 9 And it means that node 1 have the ovalization extra nodes 5 and 8. The first line of ovalization nodes includes the c1, c2 and c3 parameters, and the second line includes the d1, d2 and d3 parameters. That means that node 5 include c1, c2 and c3, and node 8 include d1, d2 and d3 for beam node 1. All ovalization dofs can be written to the ascii file “elbwov” if the correct print flag is set on *SEC- TION_BEAM. These extra nodes can be constrained as usual nodes. For exam- ple for a cantilever beam that is mounted at node 1, the nodes 1, 5 and 8 should be constrained. The ovalization is approximated with the following trigono- metric function: 𝑤(𝑟, 𝜃) = ∑ ∑ ℎ𝑘(𝑟)(𝑐𝑚 𝑘=1 𝑚=1 𝑘 cos 2𝑚𝜃 + 𝑑𝑚 𝑘 sin 2𝑚𝜃), −1 ≤ 𝑟 ≤ 1, 0 ≤ 𝜃 < 2𝜋 where hk is the interpolation function at the physical node k. The Elbow beam only supports tubular cross sections and the pipe outer radius, a, should be smaller than the pipe bend radius, R. That is a/R<<1. Moreover, the ELBOW beams have 4 stresses: axial rr-, shear rs-, shear rt- and loop- stresses. The loop stress is written at each integration point and can be visual- ized in LS-PrePost with the user fringe plot file “elbwlp.k”. NOTE that the loop-stress is not written to d3plot as default! The NEIPB flag on *DATA- BASE_EXTENT_BINARY must be set to enable d3plot support. Right now there is only basic support from the material library. The following materials are currently supported for the ELBOW beam (if requested more materials might be added in the future): *MAT_ELASTIC (MAT_001) *MAT_PLASTIC_KINEMATIC (MAT_003) *MAT_ELASTIC_PLASTIC_THERMAL (MAT_004) *MAT_VISCOELASTIC (MAT_006) *MAT_PIECEWISE_LINEAR_PLASTICITY (MAT_024) *MAT_DAMAGE_3 (MAT_153, explicit only) *MAT_CONCRETE_BEAM (MAT_195) *ELEMENT_BEAM_PULLEY Purpose: Define pulley for beam elements. This feature is implemented for truss beam elements (*SECTION_BEAM, ELFORM = 3) using materials *MAT_001 and *MAT_156, or discrete beam elements (ELFORM = 6) using *MAT_CABLE_DISCRETE_BEAM. Card 1 1 2 3 4 Variable PUID BID1 BID2 PNID Type Default I 0 I 0 I 0 I 0 5 FD F 6 FS F 7 LMIN F 8 DC F 0.0 0.0 0.0 0.0 VARIABLE DESCRIPTION PUID BID1 BID2 PNID FD FS Pulley ID. A unique number has to be used. Truss beam element 1 ID. Truss beam element 2 ID. Pulley node, NID. Coulomb dynamic friction coefficient. Optional Coulomb static friction coefficient. LMIN Minimum length, see notes below. DC Optional decay constant to allow smooth transition between the static and dynamic friction coefficient, i.e., 𝜇𝑐 = FD + (FS − FD)𝑒−DC×∣𝑣rel∣ Remarks: Remarks: Elements 1 and 2 should share a node which is coincident with the pulley node. The pulley node should not be on any beam elements. Pulleys allow continuous sliding of a truss beam element through a sharp change of angle. Two elements (1 & 2 in Figure 17-21 of *ELEMENT_SEATBELT_SLIPRING) meet at the pulley. Node 𝐵 in the beam material remains attached to the pulley node, but beam material (in the form of unstretched length) is passed from element 1 to element 2 to achieve slip. The amount of slip at each time step is calculated from the ratio of forces in elements 1 and 2. The ratio of forces is determined by the relative angle between elements 1 and 2 and the coefficient of friction, FD. The tension in the beams are taken as 𝑇1 and 𝑇2, where 𝑇2 is on the high tension side and 𝑇1 is the force on the low tension side. Thus, if 𝑇2 is sufficiently close to 𝑇1, no slip occurs; otherwise, slip is just sufficient to reduce the ratio 𝑇2/𝑇1 to 𝑒FC×𝜃, where 𝜃 is the wrap angle, see Figures 17-22 of *ELEMENT_SEATBELT_SLIPRING. The out-of-balance force at node 𝐵 is reacted on the pulley node; the motion of node 𝐵 follows that of pulley node. If, due to slip through the pulley, the unstretched length of an element becomes less than the minimum length LMIN, the beam is remeshed locally: the short element passes through the pulley and reappears on the other side . The new unstretched length of 𝑒1 is 1.1 × minimum length. The force and strain in 𝑒2 and 𝑒3 are unchanged; while the force and strain in 𝑒1 are now equal to those in 𝑒2. Subsequent slip will pass material from 𝑒3 to 𝑒1. This process can continue with several elements passing in turn through the pulley. To define a pulley, the user identifies the two beam elements which meet at the pulley, the friction coefficient, and the pulley node. If BID1 and BID2 are defined as 0 (zero), adjacent beam elements are automatically detected. The two elements must have a common node coincident with the pulley node. No attempt should be made to restrain or constrain the common node for its motion will automatically be constrained to follow the pulley node. Typically, the pulley node is part of a structure and, therefore, beam elements should not be connected to this node directly, but any other feature can be attached, including rigid bodies. *DATABASE_PLLYOUT can be used to write a time history output database pllyout for the pulley which records beam IDs, slip, slip rate, resultant force, and wrap angle. *ELEMENT_BEAM_SOURCE Purpose: Define a nodal source for beam elements. This feature is implemented only for truss beam elements (*SECTION_BEAM, ELFORM = 3) with material *MAT_001 or for discrete beam elements (ELFORM = 6) with material *MAT_071. Card 1 1 2 3 4 5 6 7 8 Variable BSID BSNID BSEID NELE LFED FPULL LMIN Type Default I 0 I 0 I 0 I 0 F F F 0.0 0.0 0.0 VARIABLE DESCRIPTION BSID Beam Source ID. A unique number has to be used. BSNID Source node ID. BSEID Source element ID. NELE LFED Number of elements to be pulled out. Beam element fed length (typical element initial length). FPULL Pull-out force. GT.0: Constant value, LT.0: Load curve ID = (-FPULL) which defines pull-out force as a function of time. Either *DEFINE_FUNCTION or *DEFINE_ CURVE_FUNCTION (with argument TIME) can be used. LMIN Minimum beam element length, see notes below. One to two tenth of the fed length LFED is usually a good choice. Remarks: The source node BSNID can be defined for itself or it can be part of another structure. It is free to move in space during the simulation process. Initially, the source node should have the same coordinates as one of the source element (BSEID) nodes, but not having the same ID. If the pre-defined pull-out force FPULL is exceeded in the element next to the source, beam material gets drawn out by increasing the length of the beam without increasing its axial force (equivalent to ideal plastic flow at a given yield force). If more than the pre-defined length LFED is drawn out, a new beam element is generated. A new beam element has an initial undeformed length of 1.1 × LMIN. The maximum number of elements NELE times the fed length LFED defines the maximum cable length that can be pulled out from the source node. The available option is: TITLE *ELEMENT_BEARING Purpose: Define a bearing between two nodes. A description of this model can be found in Carney, Howard, Miller, and Benson [2014]. Title Card. Additional card for title keyword Option. Card 1 1 2 3 4 5 6 7 8 Variable Type Default Remarks Card 1 Variable Type Default 1 ID I 0 2 ITYPE I 0 3 N1 I 0 TITLE C none 1 4 CID1 I 0 8 5 N2 I 0 6 CID2 I 0 7 NB I 0 Material Properties Card. Card 2 1 2 3 4 5 6 7 8 Variable EBALL PRBALL ERACE PRRACE STRESL Type F F F F F Default 0.0 0.0 0.0 0.0 0.0 5 6 7 8 5 6 7 8 Geometry Card. Card 3 Variable Type 1 D F 2 DI F 3 DO 4 DM F F Default 0.0 0.0 0.0 0.0 Geometry Card 2. Card 4 Variable 1 A0 Type F 2 BI F 3 BO F 4 PD F Default 0.0 0.0 0.0 0.0 Preloading Card. Card 5 1 2 3 4 5 6 7 8 Variable IPFLAG XTRAN YTRAN ZTRAN XROT YROT Type I F F F F F Default 00 0.0 0.0 0.0 0.0 0.0 VARIABLE DESCRIPTION ID Bearing ID. ITYPE Bearing type: EQ.1: ball bearing EQ.2: roller bearing N1 Node on centerline of shaft (the shaft rotates). VARIABLE DESCRIPTION CID1 N2 CID2 Coordinate ID on shaft. The local z axis defines the axis of rotation. Node on centerline of bearing (the bearing does not rotate). It should initially coincide with N1. Coordinate ID on bearing. The local z axis defines the axis of rotation. NB Number of balls or rollers. EBALL Young’s modulus for balls or rollers. PRBALL Poisson’s ratio for balls or rollers. ERACE Young’s modulus for races. PRRACE Poisson’s ratio for races. STRESL Specified value of the bearing stress required to print a warning message that the value has been reached. If it is 0.0, then no message is printed. D DI DO DM A0 BI BO PD Diameter of balls or rollers. Bore inner diameter. Bore outer diameter. Pitch diameter. If DM is not specified, it is calculated as the average of DI and DO. Initial contact angle in degrees Inner groove radius to ball diameter ratio for ball bearings and the roller length for roller bearings.. Outer race groove radius to ball diameter ratio. Unused for roller bearings. Total radial clearance between the ball bearings and races when no load is applied. VARIABLE DESCRIPTION IPFLAG Preload flag EQ.0: no preload. EQ.1: displacement preload specified. EQ.2: force preload specified. XTRAN Displacement or force preload in the local x direction. YTRAN Displacement or force preload in the local y direction. ZTRAN Displacement or force preload in the local z direction. Angle (in radians) or moment preload in local x direction. Angle (in radians) or moment preload in local y direction. XROT YROT Remarks: 1. If the bearing stress limit parameter, STRESL, is exceeded, a message is written to the messag and d3hsp files. When this value is exceeded there is no change in element behavior.s 2. Use of double precision for solution stability is strongly suggested. 3. A realistic level of bearing damping (which can be included using *ELEMENT_- DISCRETE and *MAT_DAMPER_VISCOUS) may be needed for solution stabil- ity. 4. Bearing forces can be output in the brngout file, using *DATABASE_BEARING. *ELEMENT_DIRECT_MATRIX_INPUT_{OPTION} Available options include: <BLANK> BINARY Purpose: Define an element consisting of mass, damping, stiffness, and inertia matrices in a specified file which follows the format used in the direct matrix input, DMIG, of NASTRAN. The supported format is the type 6 symmetric matrix in real double precision. LS-DYNA supports both the standard and the extended precision formats. The binary format from *CONTROL_IMPLICIT_MODES or *CONTROL_IMPLICIT_- STATIC_CONDENSATION is another input option. The mass and stiffness matrices are required. The inertia matrix is required when using *LOAD_BODY_OPTION to correctly compute the action of a prescribed base acceleration on the superelement, otherwise the inertia matrix is unused. The damping matrix is optional. The combination of these matrices is referred to as a superelement. Three input cards are required for each superelement. The degrees-of-freedom for this superelement may consist of generalized coordinates as well was nodal point quantities. Degrees-of-freedom, defined using *NODE input, are called attachment nodes. Only attachment nodes are included in the output to the ASCII and binary databases. The matrices for a given superelement can be of different order. However, the explicit integration scheme requires the inversion of the union of the element mass matrix and nodal masses associated with attachment nodes. Any degree of freedom included in the other (stiffness, damping, inertia) matrices but without nonzero columns in the combined mass matrix will be viewed as massless and constrained not to move. After deleting zero rows and columns the combined mass matrix is required to be positive definite. The inertia matrix is required to have 3 columns which corresponds to the 3 global coordinates. It is used to compute the forces acting on the superelement by multiplying the inertia matrix times the gravitational acceleration specified via *LOAD_BODY_OP- TION. There is no assumption made on the order of the matrices nor the sparse matrix structure of the element matrices except that they are symmetric and the combined mass matrix is invertible as described above. Multiple elements may be input using *ELEMENT_DIRECT_MATRIX_INPUT. They may share attachment nodes with other direct matrix input elements. Only *BOUND- ARY_PRESCRIBED_MOTION and global constraints imposed via*NODE or *BOUND- ARY_SPC on attachment nodes can be applied in explicit applications. Implicit applications can have additional constraints on attachment nodes. Card 1 1 2 3 4 5 6 7 8 Variable EID IFRMT Type I Card 2 1 0 2 Variable Type 3 4 5 6 7 8 FILENAME C Card 3 1 2 3 4 5 6 7 8 Variable MASS DAMP STIF INERT Type C C C C VARIABLE DESCRIPTION EID Super element ID. IFRMT Format: EQ.0: standard format NE.0: extended precision format MASS DAMP Name of mass matrix in the file defined by FILENAME. This filename should be no more than eight characters to be compatible with NASTRAN. Name of damping matrix in the file defined by FILENAME. This filename should be no more than eight characters to be compatible with NASTRAN. STIF *ELEMENT_DIRECT_MATRIX_INPUT DESCRIPTION Name of stiffness matrix in the file defined by FILENAME. This filename should be no more than eight characters to be compatible with NASTRAN. INERT Name of inertia matrix in the file defined by FILENAME. This filename should be no more than eight characters to be compatible with NASTRAN. This file must be present when *LOAD_BODY is used to put gravitational forces on the model. Available options include: <BLANK> LCO *ELEMENT Purpose: Define a discrete (spring or damper) element between two nodes or a node and ground. An option, LCO, is available for using a load curve(s) to initialize the offset to avoid the excitation of numerical noise that can sometimes result with an instantaneous imposition of the offset. This can be done using a single curve at the start of the calculation or two curves where the second is used during dynamic relaxation prior to beginning the transient part. In the latter case, the first curve would simply specify the offset as constant during time. If the LCO option is active, a second card is read. Beam type 6, see *ELEMENT_BEAM and SECTION_BEAM, may be used as an alternative to *ELEMENT_DISCRETE and *SECTION_DISCRETE, and is recommended if the discrete element’s line of action is not node N1 to N2, i.e., if VID.NE.0. NOTE: The discrete elements enter into the time step calcu- lations. Care must be taken to ensure that the nodal masses connected by the springs and dampers are defined and unrealistically high stiffness and damp- ing values must be avoided. All rotations are in ra- dians. Card 1 2 3 4 5 6 7 Variable EID PID N1 N2 VID Type I I I I I Default none none none none 0 S F 1. 8 PF I 0 9 10 OFFSET F Offset Load Curve Card. Additional card for LCO keyword option. Card 2 1 2 3 4 5 6 7 8 Variable LCID LCIDDR Type I I Default none none VARIABLE DESCRIPTION EID PID N1 N2 VID Element ID. A unique number is required. Since null beams are created for visualization, this element ID should not be identical to element ID’s defined for ELEMENT_BEAM and ELEMENT_- SEATBELT. Part ID, see *PART. Nodal point 1. Nodal point 2. If zero, the spring/damper connects node N1 to ground. Orientation option. The orientation option should be used cautiously since forces, which are generated as the nodal points displace, are not orthogonal to rigid body rotation unless the nodes are coincident.. The type 6, 3D beam element, is recommended when orientation is required with the absolute value of the parameter SCOOR set to 2 or 3, since this option avoids rotational constraints. EQ.0: the spring/damper acts along the axis from node N1 to N2, NE.0: the spring/damper acts along the axis defined by the orientation vector, VID defined in the *DEFINE_SD_ORI- ENTATION section. S PF Scale factor on forces. Print flag: EQ.0: forces are printed in DEFORC file, EQ.1: forces are not printed DEFORC file. VARIABLE OFFSET DESCRIPTION Initial offset. The initial offset is a displacement or rotation at time zero. For example, a positive offset on a translational spring will lead to a tensile force being developed at time zero. Ignore this input if LCID is defined below. LCID Load curve ID defining the initial OFFSET as a function of time. Positive offsets correspond to tensile forces, and, likewise negative offsets result in compressive forces. LCIDDR Load curve ID defining OFFSET as a function of time during the dynamic relaxation phase. *ELEMENT_DISCRETE_SPHERE_{OPTION} Available options include: <BLANK> VOLUME Purpose: Define a discrete spherical element for discrete element method (DEM) calculations. Currently, LS-DYNA’s implementation of the DEM supports only spherical particles, as discrete element spheres (DES). Each DES consists of a single node with its mass, mass moment of inertia, and radius defined by the input below. Initial coordinates and velocities are specified via the nodal data. The element ID corresponds to the ID of the node. The discrete spherical elements are visualized in LS- PrePost using the same options as the SPH elements. If the VOLUME option is active, the fields for MASS and INERTIA are based on per unit density. Please note, the DES part requires *PART, *SECTION, and *MAT keywords. The element type and formulation values in *SECTION are ignored. DEM retrieves the bulk modulus from the *MAT input for coupling stiffness and time step size evaluation, and density from the *MAT input if VOLUME is used to calculate the proper mass. *MAT_- ELASTIC and *MAT_RIGID are most commonly used, but other material models are also permissible. Card 1 1 2 3 4 5 6 7 8 Variable NID PID MASS/ VOLUME INERTIA RADIUS Type I I F F F Default none none none none none VARIABLE DESCRIPTION NID PID DES Node ID. DES Part ID, see *PART. VARIABLE MASS/ VOLUME DESCRIPTION If the VOLUME keyword option is set, then VOLUME and the mass is calculated from material density, Otherwise this entry is interpreted as mass. 𝑀 = MASS × 𝜌mat. INERTIA Mass moment of inertia. If the VOLUME option is active, the actual inertia is calculated from material density, 𝐼 = INERTIA × 𝜌mat. RADIUS Particle radius. The particle radius is used for defining contact between particles. *ELEMENT_GENERALIZED_SHELL Purpose: Define a general 3D shell element with an arbitrary number of nodes. The formulation of this element is specified in *DEFINE_ELEMENT_GENERALIZED_- SHELL, which is specified through the part ID and the section ID . For an illustration of this referencing, see Figure 15-31. Using this generalized shell implementation allows a rapid prototyping of new shell element formulations without further coding. The element formulation used in *SECTION_SHELL needs to be greater or equal than 1000. Card 1 1 2 3 4 5 6 7 8 Variable EID PID NMNP Type I I I Default none none none Connectivity Cards. Define the connectivity of the element by specifying NMNP- nodes (up to eight nodes per card). Include as many cards as needed. For example, for NMNP = 10, the deck should include two additional cards. Card 2 Variable 1 N1 Type I 2 N2 I 3 N3 I 4 N4 I 5 N5 I 6 N6 I 7 N7 I 8 N8 I Default none none none none none none none none VARIABLE DESCRIPTION EID PID Element ID. Chose a unique number with respect to other elements. Part ID, see *PART. NMNP Number of nodes to define this element. Ni Nodal point i (defined via *NODE) to define connectivity of this element. Remarks: 1. For post-processing and the treatment of contact boundary conditions, the use of interpolation shell elements is necessary. 2. The definition of the connectivity of the element is basically arbitrary but it has to be in correlation with the definition of the element formulation in *DEFINE_- ELEMENT_GENERALIZED_SHELL. 26 25 16 15 24 14 Connectivity of Generalized-Shell Element Generalized-Shell Element *ELEMENT_GENERALIZED_SHELL $---+--EID----+--PID----+-NMNP----+----4----+----5----+----6----+----7----+----8 1 11 $---+---N1----+---N2----+---N3----+---N4----+---N5----+---N6----+---N7----+---N8 16 $---+---N9----+--Etc----+--Etc----+--Etc----+--Etc----+--Etc----+--Etc----+--Etc 15 26 24 14 25 6 *PART Part for generalized shell $---+-- PID----+SECID----+--MID----+----4----+----5----+----6----+----7----+----8 11 15 *SECTION_SHELL $---+ SECID----ELFORM----+-SHRF----+--NIP----+----5----+----6----+----7----+----8 $---+---T1----+---T2----+---T3----+---T4----+----5----+----6----+----7----+----8 1001 15 1.0 *DEFINE_ELEMENT_GENERALIZED_SHELL $---ELFORM---+---NGP----+-NMNP----+IMASS----+-FORM----+----6----+----7----+----8 0 1001 4 9 ... Figure 17-3. Example of the connection between *ELEMENT_GENERAL- IZED_SHELL and *DEFINE_ELEMENT_GENERALIZED_SHELL. *ELEMENT_GENERALIZED_SOLID Purpose: Define a general 3D solid element with an arbitrary number of nodes. The formulation of this element is specified in *DEFINE_ELEMENT_GENERALIZED_SOL- ID, which is referenced through the part ID and the section ID . For an illustration of this referencing, see Figure 17-4. Using this generalized solid implementation allows a rapid prototyping of new solid element formulations without further coding. The element formulation used in *SECTION_SOLID needs to be greater or equal than 1000. Card 1 1 2 3 4 5 6 7 8 Variable EID PID NMNP Type I I I Default none none none Connectivity Cards. Define the connectivity of the element by specifying NMNP- nodes (up to eight nodes per card). Include as many cards as needed. For example, for NMNP = 10, the deck should include two additional cards. Card 2 Variable 1 N1 Type I 2 N2 I 3 N3 I 4 N4 I 5 N5 I 6 N6 I 7 N7 I 8 N8 I Default none none none none none none none none VARIABLE DESCRIPTION EID PID Element ID. Chose a unique number with respect to other elements. Part ID, see *PART. NMNP Number of nodes to define this element. Ni Nodal point i (defined via *NODE) to define connectivity of this element. Remarks: 1. For post-processing the use of interpolation solid elements is necessary. 2. The definition of the connectivity of the element is basically arbitrary but it has to be in correlation with the definition of the element formulation in *DEFINE_- ELEMENT_GENERALIZED_SOLID. 56 55 46 45 26 54 24 25 44 15 16 35 14 34 36 Connectivity of Generalized-Solid Element Generalized-Solid Element *ELEMENT_GENERALIZED_SOLID $---+--EID----+--PID----+-NMNP----+----4----+----5----+----6----+----7----+----8 11 18 56 $---+---N1----+---N2----+---N3----+---N4----+---N5----+---N6----+---N7----+---N8 35 46 $---+---N9----+--N10----+--N11----+--N12----+--N13----+--N14----+--N15----+--N16 24 $---+--N17----+--N18----+--Etc----+--Etc----+--Etc----+--Etc----+--Etc----+--Etc 26 55 34 25 54 36 14 44 16 45 15 5 *PART Part for generalized solid $---+--PID----+SECID----+--MID----+----4----+----5----+----6----+----7----+----8 11 15 *SECTION_SOLID $---+SECID----ELFORM----+--AET----+----4----+----5----+----6----+----7----+----8 1001 15 *DEFINE_ELEMENT_GENERALIZED_SOLID $---ELFORM---+---NGP----+-NMNP----+IMASS----+----5----+----6----+----7----+----8 1001 18 8 Figure 17-4. Example of the connection between *ELEMENT_GENERAL- IZED_SOLID and *DEFINE_ELEMENT_GENERALIZED_SOLID. Available options include: <BLANK> OFFSET *ELEMENT_INERTIA Purpose: to allow the lumped mass and inertia tensor to be offset from the nodal point. The nodal point can belong to either a deformable or rigid node. Card 1 1 2 3 4 5 6 7 8 9 10 Variable EID NID CSID Type I I I Default none none none Remarks 1 Card 2 1 Variable IXX 2 IXY 3 IXZ 4 IYY 5 IYZ 6 7 8 IZZ MASS Type F F F F F F F Default 0.0 0.0 0.0 0.0 0.0 0.0 0.0 Remarks 2 2 Offset Card. Additional card for offset keyword option. Card 3 1 2 3 4 5 6 7 8 Variable X-OFF Y-OFF Z-OFF Type F Default 0. Remarks F 0. 2 F 0. 2 VARIABLE DESCRIPTION EID NID CSID IXX IXY IXZ IYY IYZ IZZ MASS X-OFF Y-OFF Z-OFF Element ID. A unique number must be used. Node ID. Node to which the mass is assigned. Coordinate system ID EQ.0: global inertia tensor GE.1: principal moments of inertias with orientation vectors defined by Coordinate system CSID. See *DEFINE_CO- ORDINATE_SYSTEM and *DEFINE_COORDINATE_- VECTOR. 𝑥𝑥component of inertia tensor. 𝑥𝑢 component of inertia tensor. 𝑥𝑧 component of inertia tensor. 𝑦𝑦 component of inertia tensor. 𝑦𝑧 component of inertia tensor. 𝑧𝑧 component of inertia tensor. Lumped mass 𝑥-offset from nodal point. 𝑦-offset from nodal point. 𝑧-offset from nodal point. *ELEMENT_INERTIA 1. The coordinate system cannot be defined for this element using the option, *DEFINE_COORDINATE_NODE. 2. If CSID is defined then IXY, IXZ and IYZ are set to zero. The nodal inertia tensor must be positive definite, i.e., its determinant must be greater than zero, since its inverse is required. This check is done after the nodal inertia is added to the defined inertia tensor. *ELEMENT_INTERPOLATION_SHELL Purpose: With the definition of interpolation shells, the stresses and other solution variables can be interpolated from the generalized shell elements permitting the solution to be visualized using standard 4-noded shell elements with one integration point (one value of each solution variable per interpolation shell). The definition of the interpolation shells is based on interpolation nodes . The connections between these various keywords are illustrated in Figure 17-5. and Card 1 1 2 3 4 5 6 7 8 Variable EIDS EIDGS NGP Type I I I Default none none none Weighting Factor Cards. These cards set the weighting factors used for interpolating the solution onto the center of this interpolation shell. Set one weight for each of the NGP integration points. Each card can accommodate 4 points; define as many cards as necessary. As an example, for NGP = 10 three cards are required. Card 2 1 Variable IP1 2 W1 3 IP2 4 W2 5 IP3 6 W3 7 IP4 8 W4 Type I F I F I F I F Default none none none none none none none none VARIABLE EIDS DESCRIPTION Element ID of the interpolation shell. This needs to coincide with a proper definition of a 4-noded shell element (*ELEMENT_SHELL) using interpolation nodes (*CONSTRAINED_NODE_INTERPOLA- TION). EIDGS Element ID of the master element defined in *ELEMENT_GENER- ALIZED_SHELL. VARIABLE DESCRIPTION NGP Number of in-plane integration points of the master element. Integration point number (1 to NGP) in the order how they were defined in *DEFINE_ELEMENT_GENERALIZED_SHELL. Interpolation weight of integration point i. IPi Wi Remarks: 1. For each interpolation shell element, one single value (𝑣𝐼𝑆) of a solution variable is interpolated based on values at the integration points (𝑣𝑖) of the master element (*ELEMENT_GENERALIZED_SHELL) and the appropriate weighting factors (𝑤𝑖). The interpolation is computed as follows: 𝑣𝐼𝑆 = 𝑁𝐺𝑃 ∑ 𝑤𝑖𝑣𝑖 𝑖=1 . 2. To use *ELEMENT_INTERPOLATION_SHELL, ELFORM = 98 has to be used in *SECTION_SHELL 26 25 15 II IV 14 24 16 III 79 80 12 83 Connectivity of Generalized-Shell Element 78 11 81 82 13 14 84 85 Generalized-Shell Element (*ELEMENT_GENERALIZED_SHELL) 86 Integration Point Interpolation Node (*CONSTRAINED_NODE_INTERPOLATION) Interpolation Element (*ELEMENT_INTERPOLATION_SHELL) *CONSTRAINED_NODE_INTERPOLATION $---+--NID----+NUMMN----+----3----+----4----+----5----+----6----+----7----+----8 78 $---+--MN1----+---W1----+--MN2----+---W2----+--MN3----+---W3----+--MN4----+---W4 0.15 0.32 0.18 0.35 26 16 25 15 *ELEMENT_SHELL $--+-EID---+ PID---+- N1---+--N2---+--N3---+--N4---+--N5---+--N6---+--N7---+--N8 82 33 79 78 81 11 *PART Part for interpolation shell $---+--PID----+SECID----+--MID----+----4----+----5----+----6----+----7----+----8 33 45 *SECTION_SHELL $---+SECID----ELFORM----+-SHRF----+--NIP----+----5----+----6----+----7----+----8 $---+---T1----+---T2----+---T3----+---T4----+----5----+----6----+----7----+----8 98 45 1.0 *ELEMENT_INTERPOLATION_SHELL $-----EIDS---+-EIDGS----+--NGP----+----4----+----5----+----6----+----7----+----8 11 $---+--IP1---+----W1----+--IP2----+---W2----+--IP3----+---W3----+--IP4----+---W4 0.1 0.2 0.5 0.2 1 4 2 3 Figure 17-5. Example for *ELEMENT_INTERPOLATION_SHELL. *ELEMENT_INTERPOLATION_SOLID Purpose: With the definition of interpolation solids, the stresses and other solution variables can be interpolated from the generalized solid elements permitting the solution to be visualized using standard 8-noded solid elements with one integration point (one value of each solution variable per interpolation solid). The definition of the interpolation solids is based on interpolation nodes . The connection between these various keywords are illustrated in Figure17-6. and Card 1 1 2 3 4 5 6 7 8 Variable EIDS EIDGS NGP Type I I I Default none none none Weighting Factor Cards. These cards set the weighting factors used for interpolating the solution onto the center of this interpolation solid. Set one weight for each of the element’s NGP integration points. Each card can accommodate 4 points; define as many cards as necessary. As an example, for NGP = 10 three cards are required. Cards 1 Variable IP1 2 W1 3 IP2 4 W2 5 IP3 6 W3 7 IP4 8 W4 Type I F I F I F I F Default none none none none none none none none VARIABLE EIDS DESCRIPTION Element ID of the interpolation solid. This needs to coincide with a proper definition of a 8-noded solid element (*ELEMENT_SOLID) using interpolation nodes (*CONSTRAINED_NODE_INTERPOLA- TION). VARIABLE EIDGS DESCRIPTION Element ID of the master element defined in *ELEMENT_GENER- ALIZED_SOLID. NGP Number of integration points of the master element. Integration point number (1 to NGP) in the order how they were defined in *DEFINE_ELEMENT_GENERALIZED_SOLID. Interpolation weight of integration point i. IPi Wi Remarks: 1. For each interpolation solid element, one single value (𝑣𝐼𝑆) of a solution variable is interpolated based on values at the integration points (𝑣𝑖) of the master element (*ELEMENT_GENERALIZED_SOLID) and the appropriate weighting factors (𝑤𝑖). The interpolation is computed as follows: 𝑣𝐼𝑆 = 𝑁𝐺𝑃 ∑ 𝑤𝑖𝑣𝑖 𝑖=1 2. To use *ELEMENT_INTERPOLATION_SOLID, ELFORM = 98 has to be used in *SECTION_SOLID 10 VI 11 II 14 15 12 13 VII VIII IV III 16 17 18 78 80 83 79 Connectivity of Generalized-Solid Element 81 11 Generalized-Solid Element (*ELEMENT_GENERALIZED_SOLID) 85 Integration Point Interpolation Node (*CONSTRAINED_NODE_INTERPOLATION) Interpolation Element (*ELEMENT_INTERPOLATION_SOLID) 82 86 84 87 88 12 89 *ELEMENT_SOLID $--+-EID---+ PID---+- N1---+--N2---+--N3---+--N4---+--N5---+--N6---+--N7---+--N8 11 33 $--+--N1---+--N2---+- N3---+--N4---+--N5---+--N6---+--N7---+--N8---+--N9---+-N10 78 79 86 81 83 85 80 82 *PART Part for interpolation solid $---+--PID----+SECID----+--MID----+----4----+----5----+----6----+----7----+----8 33 45 *SECTION_SOLID $---+SECID----ELFORM----+--AET----+----4----+----5----+----6----+----7----+----8 45 98 *ELEMENT_INTERPOLATION_SOLID $-----EIDS---+-EIDGS----+--NGP----+----4----+----5----+----6----+----7----+----8 11 $---+--IP1---+----W1----+--IP2----+---W2----+--IP3----+---W3----+--IP4----+---W4 0.07 $---+--IP5---+----W5----+--IP6----+---W6----+--IP7----+---W7----+--IP8----+---W8 0.03 0.08 0.12 0.07 0.13 0.30 0.20 4 8 5 1 3 7 2 6 Figure 17-6. Example for *ELEMENT INTERPOLATION SOLID. *ELEMENT Purpose: This feature models a lancing process during a metal forming process by trimming along a curve. Two types of lancing, instant and progressive, are supported. This keyword is used together with *DEFINE_CURVE_TRIM_3D, and only applies to shell elements. The lanced scraps can be removed (trimming) during or after lancing when used in conjunction with *DEFINE_LANCE_SEED_POINT_COORDINATES, see Trimming. The element lancing feature is supported in LS-PrePost 4.3, under Application → MetalForming → Easy Setup. For each trim include an additional card. This input ends at the next keyword (“*”) card. Card 1 1 2 3 4 Variable IDPT IDCV IREFINE SMIN Type I I Default none none I 1 F 5 AT F 6 7 8 ENDT NTIMES CIVD F I I none none none none none VARIABLE DESCRIPTION IDPT A flag to indicate if a part to be lanced is a part or a part set. GT.0: IDPT is the PID of a part to be lanced, see *PART. LT.0: the absolute value in *SET_PART_LIST. This option allows the lancing to be performed across a tailor-welded line. the part set ID, as is IDCV IREFINE A load curve ID (the variable TCID in *DEFINE_CURVE_TRIM_- 3D) defining a lancing route . XYZ format (TCTYPE = 1) has always been supported, however, IGES format (TCTYPE = 2) is not supported until Revision 110246. Set IREFINE = 1 to refine elements along lancing route until no adapted nodes exist in the neighborhood. This feature result in a more robust lancing in the form of improved lancing boundary. Available starting in Revision 107708. Values greater than “1” are not allowed. See Figure 17-15 for an example of the mesh refinement. Minimum element characteristic length to be refined to, to be supported in the future. Currently, one level of refinement will be automatically made. Activation time for lancing operation. This variable needs to be defined for both instant and progressive lancing types . If CIVD is defined, AT becomes the distance from punch home position. Lancing end time (for progressive lancing only). If CIVD is defined, ENDT becomes the distance from punch home position. Do not define for instant lancing. A progressive lancing operation is evenly divided into NTIMES segments between AT and ENDT; within each segment lancing is done instantly. Do not define for instant lancing. ID load curve (LCID) keyword The under the *BOUNDARY_PRESCRIBED_MOTION_RIGID velocity) of the tool, with VAD = 0. kinematics (time vs. Furthermore, when this variable is used, AT and ENDT will become the distances from punch bottom position. See an example inLance-trimming with negative IDPT, IGES curve, a seed node and CIVD. the to define *ELEMENT VARIABLE SMIN AT ENDT NTIMES CIVD Remarks: Lancing the blank during forming at strategic locations under controlled conditions alleviates thinning and necking of sheet metal panels. Typically, the blank is lanced in the last few millimeters before the punch reaches its home position. Being an unstable process, lancing is not favored by all stampers, nevertheless many users have devised process which would be impossible without lancing. The benefits of lancing are illustrated in Figure 17-7. In this figure two closed-loop holes are instantly lanced each along the C-pillar top (window opening area) and bottom (window regulator area) to improve the formability at those two corners. The right panel of Figure 17-7 is lanced and suffers less thinning compared to the no-lancing case, which is shown in the left-panel. This keyword offers two types of lancing operations: 1. Instant lancing. Instant lancing cuts the sheet metal once along the defined curve at a time specified in the AT field. 2. Progressive lancing. The cut is spatially divided into NTIMES sub-lances traveling along the curve in the direction of definition. See Figure 17-10. Pro- gressive lancing starts at AT and ends at ENDT thereby achieving a gradual and even release along the curve. Modeling information: Some modeling guidelines and limitations are listed below: 1. Both closed-loop (Figure 17-8) and open-loop (Figure 17-9) lancing curves are supported. Lancing curve may not cross each other, and cross itself. 2. Since progressive lancing starts from the beginning of the curve and proceeds towards the end, the direction of the curve needs to be defined to match the direction of the physical cut (Figure 17-10). The direction can be set using LS- PrePost. The menu option GeoTol→ Measure with the Edge box checked can be used to show the direction of the curve. If the direction is not as desired, GeoTol → Rever can be used to reverse the direction. 3. The effect of NTIMES can be seen in Figure 17-11. Compared with NTIMES of 6, setting NTIMES to a value of 20 results in a smoother lancing boundary and less stress concentration along the separated route. 4. Although the IGES format curve is supported in the keyword *DEFINE_- CURVE_TRIM_3D, curves defined with the keyword and used for lancing must be specified using only the XYZ format (TCTYPE = 1 or 0). The manual entry in the keyword manual for the *INTERFACE_BLANKSIZE_DEVELOPMENT keyword outlines a procedure for converting an IGES file into the required XYZ format. Note the IGES format support for lancing is enabled starting in Revi- sion 110246. 5. The first two points and as well as the last two points of the any progressive lancing curve must be separated so that LS-DYNA can correctly determine the direction of the curve. 6. The lancing curve needs to be much longer than the element sizes in the lancing area. 7. To prevent mesh distortion at the end of the lancing route ENDT must be defined to be less than the simulation completion time (slightly less is suffi- cient). 8. As currently implemented, lancing is assumed to be in the Z-direction. This keyword does not model lancing along the draw wall with surface normals nearly perpendicular to the Z-axis. 9. Tailor-welded blanks are supported; however, the lancing route should not cross the laser line, as currently only one part can be defined with one lancing curve. 10. Both *PARAMETER and *PARAMETER_EXPRESSION are supported for BT and DT as of Revision 92335. This makes it possible for users to input distance from punch home as onset of the lancing. Refer to Figure 17-13, where a punch’s velocity profile is shown, the lancing activation time “at”, is calculated based on the distance to home, “dhome” (the shaded area), punch travel veloci- ty “vdraw”, and total simulation time “ENDTIME”. The variable CIVD imple- mented in Rev 110173 removes the need for the calculation of AT from punch distance to home. 11. Mesh adaptivity (*CONTROL_ADAPTPIVE and the parameter “ADPOPT” under *PART) must be turned on during lancing. 12. All trim curves used to define lancing routes (*DEFINE_CURVE_TRIM_3D) must be placed after all other curves in the input deck. Furthermore, no curves defined by *DEFINE_CURVE_TRIM_3D that are not used for lancing should be present anywhere in the input deck. Note this restriction is removed starting in Revision 110316. 13. Only *DEFINE_CURVE_TRIM_3D (not _NEW) is supported. If defined curve is far away from the blank it will be projected in Z-direction onto the blank. Application example: A partial deck implementing instant lancing is listed below. A blank having a PID of 8 is being lanced along curves #119 and #202 instantly at 0.05 and 0.051 seconds, respectively. *ELEMENT_LANCING $ IDPT IDCV IREFINE SMIN AT ENDT NTIMES 8 119 0.0500 8 202 0.0510 *DEFINE_CURVE_TRIM_3D $# tcid tctype tflg tdir tctol toln nseed 119 1 1 0.100 1 $# cx cy cz 172.99310 42.632320 43.736160 175.69769 -163.08299 46.547531 177.46982 -278.03793 49.138161 186.82404 -303.67191 51.217964 205.16177 -315.33484 53.299248 ⋮ ⋮ ⋮ *DEFINE_CURVE_TRIM_3D $# tcid tctype tflg tdir tctol toln nseed 202 1 1 0.100 1 $# cx cy cz 187.46982 -578.73793 89.238161 168.88404 -403.97191 61.417964 215.18177 -215.03484 73.899248 ⋮ ⋮ ⋮ A partial keyword deck implementing two progressive lances is listed below. Both lances travel along paths starting at the same coordinate value. A sheet blank having a part ID of 9 is progressively lanced along both curves (IDCV = 1 and 2) as defined by *DEFINE_CURVE_TRIM_3D. Both lancing operations commence at 0.05 seconds and finish at 0.053 seconds with 20 cuts along each curve in opposite direction. The lancing results are shown in Figure 17-12. Note that the termination time is 53.875 seconds, which is slightly larger than the ENDT. *ELEMENT_LANCING $ IDPT IDCV IREFINE SMIN AT ENDT NTIMES 9 1 0.0500 5.3E-02 20 9 2 0.0500 5.3E-02 20 *DEFINE_CURVE_TRIM_3D $# tcid tctype tflg tdir tctol toln nseed 1 1 1 0.100 1 $# cx cy cz 172.99310 42.632320 43.736160 175.69769 -163.08299 46.547531 177.46982 -278.03793 49.138161 186.82404 -303.67191 51.217964 205.16177 -315.33484 53.299248 223.13152 -308.03534 54.193089 234.96263 -290.49695 54.885273 222.03900 -270.08289 53.163551 199.31226 -251.27985 50.401234 ⋮ ⋮ ⋮ *DEFINE_CURVE_TRIM_3D 2 1 1 0.100 1 $# cx cy cz 172.99310 42.632320 43.736160 171.33121 47.22141 42.513367 171.28690 128.84601 43.032799 176.89932 149.39539 43.495331 192.41418 159.53757 44.756699 208.39861 158.93469 45.878036 218.10101 149.34409 47.128345 218.34503 135.23810 47.682144 209.05414 122.82422 46.616959 190.19659 117.66074 44.858204 ⋮ ⋮ ⋮ Trimming after lancing: removed lancing simulation. (trimming) after a As shown in Figure 17-14 and the following partial keyword file, the lanced scraps can An extra keyword, be *DEFINE_LANCE_SEED_POINT_COORDINATES is needed to define the portion that would remain after the lancing and trimming. It should be obvious that the lancing curve defined by *DEFINE_CURVE_TRIM_3D must form a closed loop. The following example will trim a part ID 9 with a fully enclosed lancing curve #1, at time = 0.049 seconds. Since the termination time is 0.0525 seconds, the scrap will be deleted (trimmed off) before the simulation ends. The scrap, enclosed by the curve, is located outside *DEFINE_LANCE_SEED_POINT_COORDINATES (starting in Revision 107262). defined node, seed the of by *CONTROL_TERMINATION 0.0525 *ELEMENT_LANCING $ IDPT IDCV IREFINE SMIN AT ENDT NTIMES 9 1 0.0490 *DEFINE_CURVE_TRIM_3D $# tcid tctype tflg tdir tctol toln nseed 1 1 1 0.100 1 $# cx cy cz 172.99310 42.632320 43.736160 175.69769 -163.08299 46.547531 177.46982 -278.03793 49.138161 186.82404 -303.67191 51.217964 205.16177 -315.33484 53.299248 223.13152 -308.03534 54.193089 ⋮ ⋮ ⋮ 172.99310 42.632320 43.736160 172.99310 42.632320 43.736160 *DEFINE_LANCE_SEED_POINT_COORDINATES $ NSEED X1 Y1 Z1 X2 Y2 Z2 1 -289.4 98.13 2354.679 This feature also makes it possible to combine the trimming process together with a forming simulation, saving a trimming step in a line-die process simulation by skipping writing out a formed dynain file and reading in the same file for the trimming simulation. Lance-trimming with negative IDPT, IGES curve, a seed node and CIVD: The following partial keyword input shows instant lance-trimming across the weld line of a tailor-welded blank using the part set ID “blksid” 100, which consists of PIDs 1 and 9. The part set ID used for *ELEMENT_LANCING input is “idpt”, which is set as the negative of blksid (-100). The lance-trimming curve ID 1117 is defined using the file lance4.iges in IGES format (TCTYPE = 2). The variable CIVD is referred to load curve ID 12, which is the kinematic curve for the punch. The lancing starts at 15.5 mm away from punch bottom (AT = 15.5). A lance seed coordinate (-382.0, -17.0, 76.0) is defined using the keyword *DEFINE_LANCE_SEED_POINT_COORDINATES, resulting in the lanced scrap piece being removed after lancing. *PARAMETER I blk1pid 1 I blk2pid 9 I blksid 100 *SET_PART_LIST &blksid &blk1pid &blk2pid *PARAMETER_EXPRESSION I idpt -1*blksid *ELEMENT_LANCING $ IDPT IDCV IREFINE SMIN AT ENDT NTIMES CIVD &idpt 1117 1 15.5 1115 *DEFINE_CURVE_TRIM_3D $# tcid tctype tflg tdir tctol toln nseed1 nseed2 1117 2 1 0 0.1000 0 lance4.iges *DEFINE_LANCE_SEED_POINT_COORDINATES $ NSUM X1 Y1 Z1 X2 Y2 Z2 1 -382.000 -17.000 76.0 *BOUNDARY_PRESCRIBED_MOTION_RIGID $ TYPEID DOF VAD LCID SF VID DEATH BIRTH &udiepid 3 0 1113 &clstime &bindpid 3 0 1114 &clstime &udiepid 3 0 1115 &endtime &clstime &bindpid 3 0 1115 &endtime &clstime Revision information: This feature is available starting in Revision 83562 for SMP and in Revision 94383 for MPP, in explicit dynamic calculation only. Later revisions incorporate various improvements. The list below provides revision information: 14. Revision 92335: support of *PARAMETER and *PARAMETER_EXPRESSION. 15. Revision 94383: MPP support of lancing is available. 16. Revision 107708: support IREFINE = 1. 17. Revision 107262: lancing with trimming is supported. 18. Revision 110173: CIVD is supported, and AT and ENDT become distances from punch home if CIVD is activated. 19. Revision 110177: support negative IDPT for part set ID, enabling lancing across the laser welded line. 20. Revision 110246: lancing curve definition in IGES format is supported. Area thinning reduced by neighboring lanced hole Thinning (%) 20.0 18.0 16.0 14.0 12.0 10.0 8.0 6.0 4.0 2.0 0.0 Area thinning reduced by neoghboring lanced hole Areas of high thinning (in blue) - without lancing Thinning contour with lancing in upper and lower C-pillar corners Figure 17-7. Thinning improvement on a door inner as a result of lancing at the upper and lower corner of the C-pillar. Figure 17-8. Instant lancing – closed-loop hole. The left mesh is immediately after AT while the right one is at punch home. Figure 17-9. Instant lancing – open-loop hole. The left mesh is immediately after AT while the right one is at punch home. ENDT Curve direction . . . AT Figure 17-10. Progressive lancing - defining AT, ENDT, NTIMES, curve direction; mesh separation progression during progressive lancing. NTIMES=6 NTIMES=20 Figure 17-11. More NTIMES gives smoother lancing boundary and less stress concentration. curve #2 direction curve #1 direction same starting point Figure 17-12. Progressive lancing – multiple lancing starting from the same coordinates. Tool velocity vdraw AT dhome Time ENDTIME *PARAMETER_EXPRESSION R dhome 12.5 R at ENDTIME-dhome/vdraw *ELEMENT_LANCING $ IDPT IDCV IREFINE SMIN AT 9 112 &at Figure 17-13. An example of defining lancing activation time AT using tool’s distance to home. Time = 0.049 Scrap deleted Time = 0.0525 Scrap kept Thinning (%) 20.0 18.0 16.0 14.0 12.0 10.0 8.0 6.0 4.0 2.0 -0.0 Seed point defines part that remains post trimming Lancing with trimming at t=0.049 sec Lancing only Figure 17-14. Lancing with trimming Lanced mesh prior to Revision 107708 Improved lanced boundary mesh with IREFINE=1 after Revision 107708 Figure 17-15. Set IREFINE = 1 (>Revision 107708) for improved lanced boundary. Available options include: <BLANK> NODE_SET *ELEMENT Purpose: Define a lumped mass element assigned to a nodal point or equally distributed to the nodes of a node set. (Note: NODE_SET option is available starting with the R3 release of Version 971.) Card 1 Variable EID Type I 2 ID I Default none none 3 4 5 6 7 8 9 10 MASS PID F 0. I none VARIABLE DESCRIPTION EID ID MASS Element ID. A unique number is recommended. The nodes in a node set share the same element ID. Node ID or node set ID if the NODE_SET option is active. This is the node or node set to which the mass is assigned. Mass value. When the NODE_SET option is active, the mass is equally distributed to all nodes in a node set. PID Part ID. This input is optional. Remarks: 1. Kinetic energy of lumped mass elements is output as kinetic energy of part 0 in matsum (*DATABASE_MATSUM) if IERODE is set to 1 on *CONTROL_OUT- PUT. *ELEMENT_MASS_MATRIX_{OPTION} Available options include: <BLANK> NODE_SET Purpose: Define a 6 × 6 symmetric nodal mass matrix assigned to a nodal point or each node within a node set. A node may not be included in more than one *ELEMENT_- MASS_MATRIX(_NODE_SET) command. Card 1 1 Variable EID Type I 2 ID I Default none none Card 2 1 2 3 CID I 0 3 4 5 6 7 8 4 5 6 7 8 Variable M11 M21 M22 M31 M32 M33 M41 Type F F F F F F F Default 0.0 0.0 0.0 0.0 0.0 0.0 0.0 Card 3 1 2 3 4 5 6 7 8 Variable M42 M43 M44 M51 M52 M53 M54 Type F F F F F F F Default 0.0 0.0 0.0 0.0 0.0 0.0 0.0 Card 4 1 2 3 4 5 6 7 8 Variable M55 M61 M62 M63 M64 M65 M66 Type F F F F F F F Default 0.0 0.0 0.0 0.0 0.0 0.0 0.0 VARIABLE DESCRIPTION EID ID CID Mij Element ID. A unique number is recommended. The nodes in a node set share the same element ID. Node ID or node set ID if the NODE_SET option is active. This is the node or node set to which the mass is assigned. Local coordinate ID which defines the orientation of the mass matrix The ijth term of the symmetric mass matrix. The lower triangular part of the matrix is defined. Available options include: <BLANK> SET *ELEMENT_MASS_PART Define additional non-structural mass to be distributed by an ar- Purpose: ea (shell) / volume (solid) or mass weighted distribution to all nodes of a given part, or part set, ID. As an option, the total mass can be defined and the additional non- structural mass is computed. This option applies to all part ID's defined by shell and solid elements. Card Variable 1 ID Type I Default none 2 3 4 5 6 7 8 9 10 ADDMASS FINMASS LCID MWD F 0. F 0. I 0 I 0 VARIABLE DESCRIPTION ID Part or part set ID if the SET option is active. A unique number must be used. ADDMASS FINMASS Added translational mass to be distributed to the nodes of the part ID or part set ID. Set to zero if FINMASS is nonzero. Since the additional mass is not included in the time step calculation of the elements in the PID or SID, ADDMASS must be greater than zero if FINMASS is zero. Final translational mass of the part ID or part set ID. The total mass of the PID or SID is computed and subtracted from the final mass of the part or part set to obtain the added translational mass, which must exceed zero. Set FINMASS to zero if ADDMASS is nonzero. FINMASS is available in the R3 release of version 971. LCID Optional load curve ID to scale the added mass at time = 0. This curve defines the scale factor as a function versus time. The curve must start at unity at t = 0. This option applies to deformable bodies only. VARIABLE MWD DESCRIPTION Optional flag for mass-weighted distribution, valid for SET option only: EQ.0: non-structural mass is distributed by ar- ea(shell)/volume(solid) weighted distribution, EQ.1: non-structural mass is distributed by mass weighted, area*density*thickness(shell)/volume*density(solid), distribution. Mixed uses with MWD for the same part should be avoided. Purpose: Define a null beam element for visualization. *ELEMENT_PLOTEL Card 1 2 3 4 5 6 7 8 9 10 Variable EID N1 N2 Type I I I Default none none none Remarks 1 VARIABLE DESCRIPTION Element ID. A unique number must be used. Nodal point (end) 1. Nodal point (end) 2. EID N1 N2 Remarks: 1. Part ID, 10000000, is assigned to PLOTEL elements. 2. PLOTEL element ID’s must be unique with respect to other beam elements. Purpose: Define a seat belt element. *ELEMENT Card 1 2 3 4 5 6 7 8 9 10 Variable EID PID N1 N2 SBRID SLEN N3 N4 Type I I I I I F Default none none none none none 0.0 Remarks 1 2 I 0 I 0 3 VARIABLE DESCRIPTION EID PID N1 N2 SBRID SLEN N3 Element ID. A unique number is required. Since null beams are created for visualization, this element ID should not be identical to element ID’s defined for ELEMENT_BEAM and ELEMENT_- DISCRETE. Part ID Node 1 ID Node 2 ID Retractor ID, see *ELEMENT_SEATBELT_RETRACTOR. Initial slack length Optional node 3 ID. When N3 > 0 and N4 > 0, the elements becomes a shell seat belt element. The thickness of the shell seatbelt is defined in *SECTION_SHELL, not in *SECTION_- SEATBELT. The shell-type seatbelt must be of a rectangular shape as shown in Figure 17-16 and contained in a logically regular mesh. N4 Node 4 ID, which is required if and only if N3 is defined. slipring retractor Top view: SN5 SRE14 SRE24 SRE13 SN4 SN3 SRE23 SRE12 SRE22 SN2 SRE11 SRE21 SN1 RN5 RE4 RN4 RE3 RN3 RE2 RN2 RE1 RN1 Figure 17-16. Definition of seatbelt shell elements. The ordering of the nodes and elements are important for seatbelt shells. See the input descriptions for SECTION_SHELL, ELEMENT_SEATBELT_RETRACTOR and ELEMENT_SEAT- BELT_SLIPRING. Remarks: 1. The retractor ID should be defined only if the element is initially inside a retractor, see *ELEMENT_SEATBELT_RETRACTOR. 2. Belt elements are single degree of freedom elements connecting two nodes. When the strain in an element is positive (i.e. the current length is greater then the unstretched length), a tension force is calculated from the material charac- teristics and is applied along the current axis of the element to oppose further stretching. The unstretched length of the belt is taken as the initial distance between the two nodes defining the position of the element plus the initial slack length. 3. Seatbelt shell elements are a new feature in version 971 and must be used with caution. The seatbelt shells distribute the loading on the surface of the dummy more realistically than the two node belt elements. For the seatbelt shells to work with sliprings and retractors it is necessary to use a logically regular mesh of quadrilateral elements. A seatbelt defined by a part ID must not be disjoint. 4. 1D and 2D seatbelt elements may not share the same material ID. *ELEMENT_SEATBELT_ACCELEROMETER Purpose: This keyword command defines an accelerometer. Contrary to the keyword name, an accelerometer need not be associated with a seat belt. The accelerometer is fixed to a rigid body containing the three nodes defined below. An accelerometer will exhibit considerably less numerical noise than a deformable node, thereby reporting more meaningful data to the user. Whenever computed accelerations are compared to experimental data, or whenever computed accelerations are compared between different runs, this feature is essential. Card 1 2 3 4 5 6 7 8 Variable SBACID NID1 NID2 NID3 IGRAV INTOPT MASS Type Default I 0 I 0 I 0 I 0 I 0 I 0 F 0. VARIABLE DESCRIPTION SBACID Accelerometer ID. A unique number must be used. NID1 NID2 NID3 Node 1 ID Node 2 ID Node 3 ID IGRAV Gravitational accelerations due to body force loads. EQ.-6: 𝑧 and 𝑥 components removed from acceleration output EQ.-5: 𝑦 and 𝑧 components removed from acceleration output EQ.-4: 𝑥 and 𝑦 components removed from acceleration output EQ.-3: 𝑧 component removed from acceleration output EQ.-2: 𝑦 component removed from acceleration output EQ.-1: 𝑥 component removed from acceleration output EQ.0: all components included in acceleration output EQ.1: all components removed from acceleration output GT.1: IGRAV is a curve ID defining the gravitation-flag versus time. The ordinate values, representing the VARIABLE DESCRIPTION gravitation-flag, can be -6, -5, -4, -3, -2, -1, 0 or 1, as de- scribed above. For example, a curve with 4 data points of (0.,1), (10.,1), (10.000001,0), (200.,0) sets gravitation flag to be 1 when time ≤ 10, and 0 when time > 10. In other words, all components of gravitational accelera- tions are removed when time ≤ 10., and then included when time > 10.0. Integration option. If the accelerometer undergoes rigid body translation without rotation this option has no effect; however, if rotation occurs, INTOPT affects how translational velocities (and displacements) are calculated. Note that the acceleration values written to the nodout file are unaffected by INTOPT. EQ.0: velocities are integrated from the global accelerations and transformed into the local system of the accelerome- ter. EQ.1: velocities are integrated directly from the local accelerations of the accelerometer. Optional added mass for accelerometer. This mass is equally distributed to nodal points NID1, NID2, and NID3. This option avoids the need to use the *ELEMENT_MASS keyword input if additional mass is required. INTOPT MASS Remarks: The presence of the accelerometer means that the accelerations and velocities of node 1 will be output to all output files in local instead of global coordinates. The local coordinate system is defined by the three nodes as follows: 1. 2. local 𝐱 from node 1 to node 2, local 𝐳 perpendicular to the plane containing nodes, 1, 2, and 3 (𝐳 = 𝐱 × 𝐚), where a is from node 1 to node 3), 3. local 𝐲 = 𝐳 × 𝐱. The three nodes should all be part of the same rigid body. The local axis then rotates with the body. *ELEMENT_SEATBELT_PRETENSIONER Purpose: Define seat belt pretensioner. A combination with sensors and retractors is also possible. Card 1 1 2 3 4 5 6 7 8 Variable SBPRID SBPRTY SBSID1 SBSID2 SBSID3 SBSID4 Type Default I 0 I 0 Remarks Card 2 1 2 I 0 1 3 I 0 I 0 I 0 4 5 6 7 8 Variable SBRID TIME PTLCID LMTFRC Type Default I 0 F 0.0 I 0 F 0 Remarks VARIABLE DESCRIPTION SBPRID Pretensioner ID. A unique number has to be used. VARIABLE DESCRIPTION SBPRTY Pretensioner type : EQ.1: pyrotechnic retractor with force limits, EQ.2: pre-loaded spring becomes active, EQ.3: lock spring removed, EQ.4: force versus time retractor. EQ.5: pyrotechnic retractor (old type in version 950) but with optional force limiter, LMTFRC. EQ.6: combination of types 4 and 5 as described in the notes below. EQ.7: independent pretensioner/retractor. EQ.8: energy versus time retractor pretensioner with optional force limiter, LMTFRC. EQ.9: energy versus time buckle or anchor pretensioner. SBSID1 Sensor 1, see *ELEMENT_SEATBELT_SENSOR. SBSID2 Sensor 2, see *ELEMENT_SEATBELT_SENSOR. SBSID3 Sensor 3, see *ELEMENT_SEATBELT_SENSOR. SBSID4 Sensor 4, see *ELEMENT_SEATBELT_SENSOR. SBRID Retractor number (SBPRTY = 1, 4, 5, 6, 7 or 8) or spring element number (SBPRTY = 2, 3 or 9). TIME Time between sensor triggering and pretensioner acting. Load curve for pretensioner (Time after activation, Pull-in) (SBPRTY = 1, 4, 5, 6, 7, 8 or 9). Optional limiting force for retractor type 5 or 8. If zero, this option is ignored. PTLCID LMTFRC Activation: To activate the pretensioner, the following sequence of events must occur: 1. Any one of up to four sensors must be triggered. 2. Then a user-defined time delay occurs. 3. Then the pretensioner acts. At least one sensor should be defined. Pretensioners allow modeling of seven types of active devices which tighten the belt during the initial stages of a crash. Types 1 and 5 implement a pyrotechnic device which spins the spool of a retractor, causing the belt to be reeled in. The user defines a pull-in versus time curve which applies once the pretensioner activates. Types 2 and 3 implement preloaded springs or torsion bars which move the buckle when released. Types 2 and 3: The pretensioner is associated with any type of spring element including rotational. Note that the preloaded spring, locking spring, and any restraints on the motion of the associated nodes are defined in the normal way; the action of the pretensioner is merely to cancel the force in one spring until (or after) it fires. With the second type, the force in the spring element is canceled out until the pretensioner is activated. In this case the spring in question is normally a stiff, linear spring which acts as a locking mechanism, preventing motion of the seat belt buckle relative to the vehicle. A preloaded spring is defined in parallel with the locking spring. This type avoids the problem of the buckle being free to ‘drift’ before the pretensioner is activated. Types 4, 6, and 7, force types, are described below. Type 1: As of version 950 the type 1 (now type 5) pretensioner requires that the user provide a load curve tabulating the pull-in of the pretensioner as a function of time. This pretensioner type interacts with the retractor, forcing it to pull in by the amount of belt indicated. It works well, and does exactly what it says it will do, but it can be difficult to use. The reason for this is that it has no regard for the forces being exerted on the belt. If a pull-in of 20mm is specified at a particular time, then 20mm of belt will be pulled in, even if this results in unrealistic forces in the seatbelt. Furthermore, there was no explicit way to turn this pretensioner off. Once defined, it overrode the retractor completely, and the amount of belt passing into or out of the retractor depended solely on the load curve specified. For the 970 release of LS-DYNA, the behavior of the type 1 pretensioner was changed due to user feedback regarding these shortcomings. Each retractor has a loading (and optional unloading) curve that describes the force on the belt element as a function of the amount of belt that has been pulled out of the retractor since the retractor locked. The new type 1 pretensioner acts as a shift of this retractor load curve. An example will make this clear. Suppose at a particular time that 5mm of belt material has left the retractor. The retractor will respond with a force corresponding to 5mm pull-out on it's loading curve. But suppose this retractor has a type 1 pretensioner defined, and at this retractor pull-out force defined force vs. time curve retractor lock time Figure 17-17 Force versus time pretensioner. At the intersection, the retractor locks. Time instant of time the pretensioner specifies a pull-in of 20mm. The retractor will then respond with a force that corresponds to (5mm + 20mm) on it's loading curve. This results in a much larger force. The effect can be that belt material will be pulled in, but unlike in the 950 version, there is no guarantee. The benefit of this implementation is that the force vs. pull-in load curve for the retractor is followed and no unrealistic forces are generated. Still, it may be difficult to produce realistic models using this option, so two new types of pretensioners have been added. These are available in 970 versions 1300 and later. Type 4: The type 4 pretensioner takes a force vs. time curve, See Figure 17-17. Each time step, the retractor computes the desired force without regard to the pretensioner. If the resulting force is less than that specified by the pretensioner load curve, then the pretensioner value is used instead. As time goes on, the pretensioner load curve should drop below the forces generated by the retractor, and the pretensioner is then essentially inactive. This provides for good control of the actual forces, so no unrealistic values are generated. The actual direction and amount of belt movement is unspecified, and will depend on the other forces being exerted on the belt. This is suitable when the force the pretensioner exerts over time is known. *ELEMENT_SEATBELT_PRETENSIONER The type 5 pretensioner is essentially the same as the old type 1 pretensioner, but with the addition of a force limiting value. The pull-in is given as a function of time, and the belt is drawn into the retractor exactly as desired. However, if at any point the forces generated in the belt exceed the pretensioner force limit, then the pretensioner is deactivated and the retractor takes over. In order to prevent a large discontinuity in the force at this point, the loading curve for the retractor is shifted (in the abscissa) by the amount required to put the current (pull-out, force) on the load curve. For example, suppose the current force is 1000, and the current pull-out is -10 (10mm of belt has been pulled IN by the pretensioner). If the retractor would normally generate a force of 1000 after 25mm of belt had been pulled OUT, then the load curve is shifted to the left by 35, and remains that way for the duration of the calculation. So that at the current pull-in of 10, it will generate the force normally associated with a pull out of 25. If the belt reaches a pull out of 5, the force will be as if it were pulled out 40 (5 + the shift of 35), and so on. This option is included for those who liked the general behavior of the old type 1 pretensioner, but has the added feature of the force limit to prevent unrealistic behavior. Type 6: The type 6 pretensioner is a variation of the type 4 pretensioner, with features of the type 5 pretensioner. A force vs. time curve is input and the pretensioner force is computed each cycle. The retractor linked to this pretensioner should specify a positive value for PULL, which is the distance the belt pulls out before it locks. As the pretensioner pulls the belt into the retractor, the amount of pull-in is tracked. As the pretensioner force decreases and drops below the belt tension, belt will begin to move back out of the retractor. Once PULL amount of belt has moved out of the retractor (relative to the maximum pull in encountered), the retractor will lock. At this time, the pretensioner is disabled, and the retractor force curve is shifted to match the current belt tension. This shifting is done just like the type 5 pretensioner. It is important that a positive value of PULL be specified to prevent premature retractor locking which could occur due to small outward belt movements generated by noise in the simulation. Type 7: The type 7 pretensioner is a simple combination of retractor and pretensioner. It is similar to the type 6 except for the following changes: when the retractor locks, the pretensioner is NOT disabled – it continues to exert force according to the force vs. time curve until the end of the simulation. (The force vs. time curve should probably drop to 0 at some time.) Furthermore, the retractor load curve is not shifted – the retractor begins to exert force according to the force vs. pull-out curve. These two forces are added together and applied to the belt. Thus, the pretensioner and retractor are essentially independent. Type 8: The type 8 pretensioner is a variation of type 5 pretensioner. The pretension energy, instead of pull-in for type 5, is given as a function of time. This enables users to use a single pretensioner curve, PTLCID, for various sizes of dummies. The energy could be yielded from the baseline test or simulation by𝐸(𝑡) = ∫ 𝑓𝑑𝑝 , where f is the force of the mouth element of the retractor and dp is the incremental pull-in. Type 9: The type 9 pretensioner is designed for a pretension-energy based buckle or anchor pretensioner. The pretensioner is modeled as a spring element, SBRID. One end of the spring element is attached to the vehicle. For a buckle pretensioner, the other end of SBRID is the slip ring node, SBRNID, of a slip ring representing the buckle. For an anchor pretensioner, SBRID shares the other end with a belt element, see Figure *ELEMENT_SEATBELT_RETRACTOR Purpose: Define seat belt retractor. See remarks below for seatbelt shell elements. Card 1 1 2 3 4 5 6 7 8 Variable SBRID SBRNID SBID SID1 SID2 SID3 SID4 Type Default I 0 I 0 Remarks 1,2 Card 2 1 2 I 0 2 3 I 0 3 4 I 0 I 0 I 0 5 6 7 8 Variable TDEL PULL LLCID ULCID LFED Type F F Default 0.0 0.0 Remarks F 0.0 I 0 4 I 0 5 VARIABLE DESCRIPTION SBRID Retractor ID. A unique number has to be used. SBRNID Retractor node ID SBID SID1 SID2 SID3 SID4 Seat belt element ID Sensor ID 1 Sensor ID 2 Sensor ID 3 Sensor ID 4 Before Element 1 Element 1 Element 2 Element 4 Element 3 Element 2 After Element 3 Element 4 Element 4 Element 4 All nodes within this area are coincident Figure 17-18. Elements in a retractor. VARIABLE DESCRIPTION TDEL PULL Time delay after sensor triggers. Amount of pull-out between time delay ending and retractor locking, a length value. LLCID Load curve for loading (Pull-out, Force), see Figure 17-18. ULCID Load curve for unloading (Pull-out, Force), see Figure 17-18. LFED Fed length, see explanation below. Remarks: 1. The retractor node should not be on any belt elements. The element defined should have one node coincident with the retractor node but should not be inside the retractor. 2. When SBRNID < 0, this retractor is for shell-type seatbelt, -SBRNID is the *SET_NODE containing RN1, RN2, …RN5. SBID is then *SET_SHELL_LIST. Note that the numbering of –SBRNID, SBID has to be consistent in the direction of numbering. For example, if *SET_NODE for SBRNID has nodes of (RN1, RN2, RN3, RN4, RN5) then *SET_SHELL_LIST for SBID should have elem. of (RE1, RE2, RE3, RE4). See Figure 17-16. 3. At least one sensor should be defined. 4. The first point of the load curve should be (0, Tmin). Tmin is the minimum tension. All subsequent tension values should be greater than Tmin. 5. The unloading curve should start at zero tension and increase monotonically (i.e., no segments of negative or zero slope). Retractors allow belt material to be paid out into a belt element. Retractors operate in one of two regimes: unlocked when the belt material is paid out, or reeled in under constant tension and locked when a user defined force-pullout relationship applies. The retractor is initially unlocked, and the following sequence of events must occur for it to become locked: a) Any one of up to four sensors must be triggered. (The sensors are de- scribed below.) b) Then a user-defined time delay occurs. c) Then a user-defined length of belt must be paid out (optional). d) Then the retractor locks and once locked, it remains locked. In the unlocked regime, the retractor attempts to apply a constant tension to the belt. This feature allows an initial tightening of the belt and takes up any slack whenever it occurs. The tension value is taken from the first point on the force- pullout load curve. The maximum rate of pull out or pull in is given by 0.01 × fed length per time step. Because of this, the constant tension value is not al- ways achieved. In the locked regime, a user-defined curve describes the relationship between the force in the attached element and the amount of belt material paid out. If the tension in the belt subsequently relaxes, a different user-defined curve ap- plies for unloading. The unloading curve is followed until the minimum ten- sion is reached. The curves are defined in terms of initial length of belt. For example, if a belt is marked at 10mm intervals and then wound onto a retractor, and the force re- quired to make each mark emerge from the (locked) retractor is recorded, the curves used for input would be as follows: 0 Minimum tension (should be > zero) 10mm Force to emergence of first mark 20mm Force to emergence of second mark ⋮ Pyrotechnic pretensions may be defined which cause the retractor to pull in the belt at a predetermined rate. This overrides the retractor force-pullout relation- ship from the moment when the pretensioner activates. If desired, belt elements may be defined which are initially inside the retractor. These will emerge as belt material is paid out, and may return into the retractor if sufficient material is reeled in during unloading. Elements e2, e3 and e4 are initially inside the retractor, which is paying out material into element e1. When the retractor has fed Lcrit into e1, where Lcrit = fed length - 1.1 × minimum length (minimum length defined on belt material input) (fed length defined on retractor input) Element e2 emerges with an unstretched length of 1.1 x minimum length; the unstretched length of element e1 is reduced by the same amount. The force and strain in e1 are unchanged; in e2, they are set equal to those in e1. The retractor now pays out material into e2. If no elements are inside the retractor, e2 can continue to extend as more mate- rial is fed into it. As the retractor pulls in the belt (for example, during initial tightening), if the unstretched length of the mouth element becomes less than the minimum length, the element is taken into the retractor. To define a retractor, the user enters the retractor node, the ‘mouth’ element (into which belt material will be fed), e1 in Figure 17-18, up to 4 sensors which can trigger unlocking, a time delay, a payout delay (optional), load and unload curve numbers, and the fed length. The retractor node is typically part of the vehicle structure; belt elements should not be connected to this node directly, but any other feature can be attached including rigid bodies. The mouth ele- ment should have a node coincident with the retractor but should not be inside the retractor. The fed length would typically be set either to a typical element initial length, for the distance between painted marks on a real belt for compari- sons with high speed film. The fed length should be at least three times the minimum length. with weblockers without weblockers Figure 17-19. Retractor force pull characteristics. Pullout If there are elements initially inside the retractor (e2, e3 and e4 in the Figure) they should not be referred to on the retractor input, but the retractor should be identified on the element input for these elements. Their nodes should all be coincident with the retractor node and should not be restrained or constrained. Initial slack will automatically be set to 1.1 × minimum length for these ele- ments; this overrides any user-defined value. Weblockers can be included within the retractor representation simply by enter- ing a ‘locking up’ characteristic in the force pullout curve, see Figure 17-19. The final section can be very steep (but must have a finite slope). 6. In an event when only retractors are used in the model, be aware that the pull- out is measured from the point when the retractor is locked. If the belt has been pulled IN since the retractor was locked, then minimum force will be seen in the retractor until the system pays out enough belt to get back to the point when locked If the behavior described in the above note undesirable then the type 6 preten- sioner model is recommended for the seat belt system. A constant force vs. time load curve with a force equal to minimum tension fwill be defined, with a small PULL value on the retractor. With this set up, the pretensioner will be active until the belt pulls all the way in, but as soon as the belt starts to move back out, the pretensioner will get disabled and the retractor will take over. *ELEMENT Purpose: Define seat belt sensor. Four types are possible, see explanation below. Card 1 1 2 3 4 5 6 7 8 Variable SBSID SBSTYP SBSFL Type Default I 0 I 0 I 0 Remarks Additional card for SBSTYP = 1. Card 2 1 2 3 4 5 6 7 8 Variable NID DOF ACC ATIME Type Default Remarks I 0 1 I 0 F F 0.0 0.0 Additional card for SBSTYP = 2. Card 2 1 2 3 4 5 6 7 8 Variable SBRID PULRAT PULTIM Type Default I 0 F F 0.0 0.0 Remarks Additional card for SBSTYP = 3. Card 2 1 2 3 4 5 6 7 8 Variable TIME Type F Default 0.0 Remarks Additional card for SBSTYP = 4. Card 2 1 2 3 4 5 6 7 8 Variable NID1 NID2 DMX DMN Type Default I 0 I 0 F F 0.0 0.0 Remarks 2 2 VARIABLE DESCRIPTION SBSID Sensor ID. A unique number has to be used. SBSTYP Sensor type: EQ.1: acceleration of node, EQ.2: retractor pull-out rate, EQ.3: time, EQ.4: distance between nodes. SBSFL Sensor flag: EQ.0: sensor active during dynamic relaxation, EQ.1: sensor can be triggered during dynamic relaxation. VARIABLE DESCRIPTION NID DOF Node ID of sensor Degree of freedom: EQ.1: x, EQ.2: y, EQ.3: z. ACC Activating acceleration ATIME Time over which acceleration must be exceeded SBRID Retractor ID, see *ELEMENT_SEATBELT_RETRACTOR. PULRAT Rate of pull-out (length/time units) PULTIM Time over which rate of pull-out must be exceeded Time at which sensor triggers Node 1 ID Node 2 ID Maximum distance Minimum distance TIME NID1 NID2 DMX DMN Remarks: 1. Node should not be on rigid body, velocity boundary condition, or other ‘imposed motion’ feature. 2. Sensor triggers when the distance between the two nodes is d > dmax or d < dmin. Sensors are used to trigger locking of retractors and activate preten- sioners. Four types of sensors are available which trigger according to the fol- lowing criteria: Type 1 When the magnitude of x-, y-, or z- acceleration of a given node has remained above a given level continuously for a given time, the sensor triggers. This does not work with nodes on rigid bodies. Type 2 When the rate of belt payout from a given retractor has remained above a given level continuously for a given time, the sensor trig- gers. Type 3 The sensor triggers at a given time. Type 4 The sensor triggers when the distance between two nodes exceeds a given maximum or becomes less than a given minimum. This type of sensor is intended for use with an explicit mass/spring represen- tation of the sensor mechanism. By default, the sensors are inactive during dynamic relaxation. This allows initial tightening of the belt and positioning of the occupant on the seat without locking the retractor or firing any pretensioners. However, a flag can be set in the sensor input to make the sensors active during the dynamic relaxation phase. *ELEMENT_SEATBELT_SLIPRING Purpose: Define seat belt slip ring. Card 1 2 3 Variable SBSRID SBID1 SBID2 Type Default I 0 I 0 I 0 4 FC F 0.0 5 6 7 8 SBRNID LTIME FCS ONID I 0 F F 1020 0.0 I 0 Optional Card. Card 2 Variable Type 1 K F Default 0.0 VARIABLE SBSRID SBID1 SBID2 FC 2 3 4 5 6 7 8 FUNCID DIRECT DC LCNFFD LCNFFS I 0 I 0 F 0 I 0 I 0 DESCRIPTION Slip ring ID. A unique number has to be used. See remarks below for the treatment of slip rings for shell belt elements. Seat belt element 1 ID Seat belt element 2 ID Coulomb dynamic friction coefficient. If less than zero, |FC| refers to a curve which defines the dynamic friction coefficient as a function of time. SBRNID Slip ring node, NID LTIME Slip ring lockup time. After this time no material is moved from one side of the slip ring to the other. This option is not active during dynamic relaxation. FCS *ELEMENT_SEATBELT_SLIPRING DESCRIPTION Optional Coulomb static friction coefficient. If less than zero, |FCS| refers to a curve which defines the static friction coefficient as a function of time. ONID Optional orientation node ID. K Optional coefficient for determining the Coulomb friction coefficient related to angle alpha FUNCID Function ID to determine friction coefficient. DIRECT Direction of belt movement: EQ.0: if the belt can move along both directions. EQ.12: if the belt is only allowed to slip along the direction from SBID1 to SBID2 EQ.21: if the belt is only allowed to slip along the direction from SBID2 to SBID DC Optional decay constant to allow a smooth transition between the static and dynamic friction coefficients, i.e., 𝜇𝑐 = FC + (FCS − FC)𝑒−DC×∣𝑣rel∣ LCNFFD LCNFFS Optional curve for normal-force-dependent Coulomb dynamic friction coefficient. friction coefficient becomes FC + 𝑓LCNFFD(𝐹𝑛), where 𝑓LCNFFD(𝐹𝑛) is the function value of LCNFFD at contact force 𝐹𝑛. When defined, the dynamic Optional curve for normal-force-dependent Coulomb static friction coefficient. When defined, the static friction coefficient becomes FCS + 𝑓LCNFFS(𝐹𝑛), where 𝑓LCNFFS(𝐹𝑛) is the function value of LCNFFS at contact force 𝐹𝑛. Slipring Node Orientation Node Figure 17-20. Orientation node. Remarks: When SBRNID < 0, this slipring is for shell-type seatbelt, -SBRNID is the *SET_NODE containing SN1, SN2, …SN5. SBID1 and SBID2 are then *SET_SHELL_LIST. Note that the numbering of -SBRNID, SBID1 and SBID2 has to be consistent in the direction of numbering. For example if, *SET_NODE for SBRNID has nodes of (SN1, SN2, SN3, SN4, SN5) then *SET_SHELL_LIST for SBID1 should have elem. of (SRE11, SRE12, SRE13, SRE14) and *SET_SHELL_LIST for SBID2 should have elem. of (SRE21, SRE22, SRE23, SRE24). See Figure 17-20. Elements 1 and 2 should share a node which is coincident with the slip ring node. Elements 1 and 2 should not be referenced in any other slipring definition. The slip ring node should not be on any belt elements. Sliprings allow continuous sliding of a belt through a sharp change of angle. Two elements (1 & 2 in Figure 17-21) meet at the slipring. Node B in the belt material Slipring Element 2 Element 1 Element 3 Element 1 Element 2 Element 3 Before After Figure 17-21. Elements passing through slipring. remains attached to the slipring node, but belt material (in the form of unstretched length) is passed from element 1 to element 2 to achieve slip. The amount of slip at each time step is calculated from the ratio of forces in elements 1 and 2. The ratio of forces is determined by the relative angle between elements 1 and 2 and the coefficient of friction, FC. The tension in the belts are taken as 𝑇1 and 𝑇2, where 𝑇2 is on the high tension side and 𝑇1 is the force on the low tension side. Thus, if 𝑇2 is sufficiently close to 𝑇1, no slip occurs; otherwise, slip is just sufficient to reduce the ratio 𝑇2/𝑇1 to 𝑒FC×𝜃, where 𝜃 is the wrap angle, see Figures 17-20 and 17-22 No slip occurs if both elements are slack. The out-of-balance force at node B is reacted on the slip ring node; the motion of node B follows that of slip ring node. If, due to slip through the slip ring, the unstretched length of an element becomes less than the minimum length (as entered on the belt material card), the belt is remeshed locally: the short element passes through the slip ring and reappears on the other side . The new unstretched length of element 1 is 1.1 × minimum length. Force and strain in elements 2 and 3 are unchanged; force and strain in element 1 are now equal to those in element 2. Subsequent slip will pass material from element 3 to element 1. This process can continue with several elements passing in turn through the slip ring. To define a slip ring, the user identifies the two belt elements which meet at the slip ring, the friction coefficient, and the slip ring node. The two elements must have a common node coincident with the slip ring node. No attempt should be made to restrain or constrain the common node for its motion will automatically be constrained to follow the slip ring node. Typically, the slip ring node is part of the vehicle body structure and, therefore, belt elements should not be connected to this node directly, but any other feature can be attached, including rigid bodies. If K is undefined, the limiting force ratio is taken as 𝑒FC×𝜃. If K is defined, the maximum force ratio is computed as 𝑒FC×𝜃(1+K×𝛼2) where alpha is the angle shown in Figure 17-23. The function is defined using the *DE- FINE_FUNCTION keyword input. This function is a function of three variables, and the ratio is given by evaluating 𝑇2 𝑇1 = FUNC(FCT, 𝜃, 𝛼) where FCT is the instantaneous friction coefficient at time 𝑡, i.e. it has the value of FC if the belt has moved in the last time-step and the value of FCS if the belt has been stationary. For example, the default behavior can be obtained using the function definition (assuming FCT has a value of 0.025 and the function ID is unity) *DEFINE_FUNCTION 1, f(fct,theta,alpha) = exp(0.025*theta) Behavior like default option can be obtained with (K=0.1): *DEFINE_FUNCTION 1, f(fct,theta,alpha) = exp(0.025*theta*(1.+0.1*alpha*alpha)) Figure 17-22. Front view showing wrap angle. Figure 17-23. Top view shows orientation of belt relative to axis. *ELEMENT_SHELL_{OPTION} Available options include: <BLANK> THICKNESS BETA or MCID OFFSET DOF COMPOSITE COMPOSITE_LONG SHL4_TO_SHL8 Stacking of options, e.g., THICKNESS_OFFSET, is allowed in some cases. When combining options in this manner, check d3hsp to confirm that all the options are acknowledged. Purpose: Define three, four, six, and eight node elements including 3D shells, membranes, 2D plane stress, plane strain, and axisymmetric solids. The type of the element and its formulation is specified through the part ID and the section ID . Also, the thickness of each element can be specified when applicable on the element cards or else a default thickness value is used from the section definition. For orthotropic and anisotropic materials, a local material angle (variable BETA) can be defined which is cumulative with the integration point angles specified in *SECTION_- SHELL, *PART_COMPOSITE, *ELEMENT_SHELL_COMPOSITE, or *ELEMENT_- SHELL_COMPOSITE_LONG. Alternatively, the material coordinate system can be defined as the projection of a local coordinate system, MCID, onto the shell. An offset option, OFFSET, is available for moving the shell reference surface from the nodal points that define the shell. The COMPOSITE or COMPOSITE_LONG option allows an arbitrary number of integration points across the thickness of shells sharing the same part ID. This is independent of thickness defined in *SECTION_SHELL. To maintain a direct association of through-thickness integration point numbers with physical plies in the case where the number of plies varies from element to element, see Remark 12. The option, SHL4_TO_SHL8, converts 3 node triangular and 4 node quadrilateral shell elements to 6 node triangular and 8 node quadrilateral quadratic shell elements, respectively, by the addition of mid-side nodal points. See Remark 9 below. For the shell formulation that uses additional nodal degrees-of-freedom, the option DOF is available to connect the nodes of the shell to corresponding scalar nodes. Four scalar nodes are required for element type 25 to model the thickness changes that require 2 additional degrees-of-freedom per shell node. Defining these nodes is optional, if left undefined, they will be automatically created. Card 1 1 2 3 4 5 6 7 8 9 Variable EID PID N1 N2 N3 N4 N5 N6 N7 Type I I I I I I I Default none none none none none none 0 I 0 I 0 10 N8 I 0 Remarks 3 3 3 3 Thickness Card. Additional card for THICKNESS, BETA, and MCID keyword options. Card 2 1 2 3 4 5 6 7 8 9 10 Variable THIC1 THIC2 THIC3 THIC4 BETA or MCID Type Default Remarks F 0. 1 F 0. F 0. F 0. F 0. Thickness Card. Additional card for THICKNESS, BETA, and MCID keyword options, is only required if mid-side nodes are defined (N5-N8).. Card 2 1 2 3 4 5 6 7 8 9 10 Variable THIC5 THIC6 THIC7 THIC8 Type Default Remarks F 0. 6 F 0. F 0. F 0. . Offset Card. Additional card for OFFSET keyword options. Card 2 1 2 3 4 5 6 7 8 9 10 Variable OFFSET Type Default Remarks F 0. Scalar Node Card. Additional card for DOF keyword option. Card 2 1 2 3 4 5 6 7 8 9 10 Variable NS1 NS2 NS3 NS4 Type Default I I I I Remarks 8 8 8 8 COMPOSITE Cards. Additional set of cards for the COMPOSITE keyword option. Set the material ID, thickness, and material angle for each through-thickness integration point of a composite shell are provided below (up to two integration points per card). The integration point data should be given sequentially starting with the bottommost integration point. The total number of integration points is determined by the number of entries on these cards. The thickness of each shell is the summation of the integration point thicknesses. Define as many cards as needed. Card 2 1 2 Variable MID1 THICK1 Type I F 3 B1 F 4 5 6 MID2 THICK2 I F 8 7 B2 F COMPOSITE_LONG Cards. Additional set of cards for the COMPOSITE_LONG keyword option. Set the material ID, thickness, and material angle for each through- thickness integration point of a composite shell are provided below (one integration point per card). The integration point data should be given sequentially starting with the bottommost integration point. The total number of integration points is determined by the number of entries on these cards. The thickness of each shell is the summation of the integration point thicknesses. Define as many cards as needed. Column 4 must be left blank. Card 2 1 2 Variable MID1 THICK1 Type I F 3 B1 F 4 5 6 7 8 PLYID1 VARIABLE DESCRIPTION EID PID N1 N2 N3 N4 N5-N8 THIC1 THIC2 THIC3 THIC4 BETA THIC5 THIC6 THIC7 THIC8 MCID Element ID. Chose a unique number with respect to other elements. Part ID, see *PART. Nodal point 1 Nodal point 2 Nodal point 3 Nodal point 4 Mid-side nodes for eight node shell Shell thickness at node 1 Shell thickness at node 2 Shell thickness at node 3 Shell thickness at node 4 Orthotropic material base offset angle . The angle is given in degrees. If blank the default is set to zero. Shell thickness at node 5 Shell thickness at node 6 Shell thickness at node 7 Shell thickness at node 8 Material coordinate system ID. The a-axis of the base (or element- level) material coordinate system is the projection of the x-axis of coordinate system MCID onto the surface of the shell element. The c-axis of the material coordinate system aligns with the shell normal. The b-axis is taken as b = c x a. Each layer in the element can have a unique material orientation by defining a rotation angle for each layer as described in Remark 5. n1 n1 n3 n2 *ELEMENT_SHELL n3 n3 Figure 17-24. LS-DYNA shell elements. Counterclockwise node numbering determines the top surface. OFFSET The offset distance from the plane of the nodal points to the reference surface of the shell in the direction of the normal vector to the shell. NS1 NS2 NS3 NS4 MID Scalar node 1, parameter NDOF on the *NODE_SCALAR is normally set to 2. If the thickness is constrained, set NDOF = 0. Scalar node 2 Scalar node 3 Scalar node 4 Material ID of integration point 𝑖, see *MAT_… Section. THICK Thickness of integration point 𝑖. B Material angle of integration point 𝑖. PLYID Ply ID for integration point 𝑖 (for post-processing purposes). Remarks: 1. Default Thickness. Default values in place of zero shell thicknesses are taken from the cross-section property definition of the PID, see *SECTION_SHELL. 2. Ordering. Counterclockwise node numbering determines the top surface, see Figure 17-24 3. Coordinate Systems. Stresses and strain output in the binary databases are given in the global coordinate system, whereas stress resultants are output in the local coordinate system for the shell element. 4. Convexity. Interior angles must be less than 180 degrees. 5. Material Orientation. To allow the orientation of orthotropic and anisotropic materials to be defined for each shell element, a BETA angle can be defined. This BETA angle is used with the AOPT parameter and associated data on the *MAT card to determine an element reference direction for the element. The AOPT data defines a coordinate system and the BETA angle defines a subse- quent rotation about the element normal to determine the element reference system. For composite modeling, each layer in the element can have a unique material direction by defining an additional rotation angle for the layer, using either the ICOMP and B𝑖 parameters on *SECTION_SHELL or the B𝑖 parameter on *PART_COMPOSITE. The material direction for layer 𝑖 is then determined by a rotation angle, 𝜃𝑖 as shown in Figures 17-25 and 17-26. i = β+β Figure 17-25. A multi-layer laminate can be defined. The angle β for the i’th lamina (integration point), see *SECTION_SHELL. i is defined n4 n2 n3 n1 Figure 17-26. Orientation of material directions (shown relative to the 1-2 side as when AOPT = 0 in *MAT). 6. Activation of the BETA Field and Its Interpretation. To activate the BETA field, either the BETA or THCKNESS keyword option must be used. There is a difference in how a zero value or empty field is interpreted. When the BETA keyword option is used, a zero value or empty BETA field will override the BETA on *MAT. However, when the THICKNESS keyword option is used, a zero value or empty BETA field will not override the BETA value on *MAT. Therefore, to input BETA=0, the BETA keyword option is recommended. If a THIC value is omitted or input as zero, the thickness will default to the value on the *SECTION_SHELL card. If mid-side nodes are defined (N5-N8), then a second line of thickness values will be read. This line may be left blank, but cannot be omitted. 7. Offset for the Reference Surface. The parameter OFFSET gives the offset from the nodal points of the shell to the reference surface. This option applies to most shell formulations excluding two-dimensional elements, membrane elements, and quadratic shell elements. Except for Mortar contacts, the refer- ence surface offset given by OFFSET is not taken into account in the contact subroutines unless CNTCO is set to 1 in *CONTROL_SHELL. For Mortar con- tacts the OFFSET determines the location of the contact surface. 8. Scalar Nodes. The scalar nodes specified on the optional card refer to the scalar nodes defined by the user to hold additional degrees of freedom for shells with this capability. Scalar nodes are used with shell element type 25 and 26. 9. Automatic Order Increase. The option, SHL4_TO_SHL8, converts 3 node triangular and 4 node quadrilateral shell elements to 6 node triangular and 8 node quadrilateral quadratic shell elements, respectively, by the addition of mid-side nodal points. The user node ID’s for these generated nodes are offset after the largest user node ID defined in the input file. When defining the *SEC- TION_SHELL keyword, the element type must be specified as either 23 or 24 corresponding to quadratic quadrilateral and triangular shells, respectively. 10. Cohesive Elements. Cohesive elements (ELFORM=29, 46 or 47 on *SEC- TION_SHELL) may be defined with zero depth to connect surfaces with no gap between them, but must have nodes 1 and 2 on one surface and nodes 3 and 4 on the other. 11. Contact Thickness when using *ELEMENT_SHELL_THICKNESS in MPP. When using MPP, THEORY = 1 in *CONTROL_SHELL has special meaning when dealing with non-uniform-thickness shells, that is, it serves to set the nodal contact thickness equal to the average of the nodal thicknesses from the shells sharing that node. Thus when a contact surface is comprised of non- uniform-thickness shells, THEORY = 1 is recommended and the user still has the option of setting the actual shell theory using ELFORM in *SECTION_- SHELL. 12. Assignment of Zero Thickness to Integration Points. The ability to assign zero- thickness integration points in the stacking sequence allows the number of integration points to remain constant even as the number of physical plies var- ies from element to element and eases post-processing since a particular inte- gration point corresponds to a physical ply. Such a capability is important when one or more of the physical plies are not continuous across a part. To represent a missing ply in *ELEMENT_SHELL_COMPOSITE, set THICKi to 0.0 for the corresponding integration point and additionally, either set MID=-1 or, if the LONG option is used, set PLYID to any nonzero value. When postprocessing the results using LS-PrePost version 4.5, read both the keyword deck and d3plot database into the code and then select Option > N/A gray fringe. Then, when viewing fringe plots for a particular integration point (FriComp > IPt > intpt#), the element will be grayed out if the selected integra- tion point is missing (or has zero thickness) in that element. *ELEMENT_SHELL_NURBS_PATCH Purpose: Define a NURBS-surface element (patch) based on a rectangular grid of control points. This grid consists of NPR*NPS control points, where NPR and NPS are the number of control points in local r- and s-direction, respectively. The necessary shape functions are defined through two knot-vectors: 1. Knot-Vector in r-direction with length NPR + PR + 1 and 2. Knot-Vector in s-direction with length NPS + PS + 1 There is no limit on the size of the underlying grid to define a NURBS-surface element, so the total number of necessary Keyword-cards depends on the parameters given in the first two cards and is given by # of cards = 2 + ⌈ NPR + PR + 1 ⌉ + ⌈ NPS + PS + 1 ⌉ + NPS × ⌈ NPR ⌉, where ⌈𝑥⌉ = ceil(𝑥). (NOTE: the last term in the sum is doubled if WFL = 1, indicating that the weights are user-specified). An example partial keyword deck using this card is given in Figure 17-28. Card 1 1 2 3 Variable NPID PID NPR Type I I I 4 PR I 5 NPS I 6 PS I 7 8 Default none none none none none none Card 2 1 2 3 4 5 6 Variable WFL FORM INT NISR NISS IMASS Type Default I 0 I 0 I 0 I I PR PS I 0 8 7 NL I 0 Remarks Figure 17-28 Figure 17-28 Knot Vector Cards (for r-direction). The knot-vector in local r-direction with length NPR +PR + 1 is given below (up to eight values per card) requiring a total of Ceil[ (NPR +PR + 1)/8 ] cards. Cards A 1 2 3 4 5 6 7 8 Variable RK1 RK2 RK3 RK4 RK5 RK6 RK7 RK8 Type F F F F F F F F Default none none none none none none none none Knot Vector Cards (for s-direction). The knot-vector in local s-direction with length NPS +PS + 1 is given below (up to eight values per card) requiring a total of Ceil[ (NPS +PS + 1)/8 ] cards. Cards B 1 2 3 4 5 6 7 8 Variable SK1 SK2 SK3 SK4 SK5 SK6 SK7 SK8 Type F F F F F F F F Default none none none none none none none none Connectivity Cards. The connectivity of the control grid is a two dimensional table of NPS rows and NPR columns. This data fills NPS sets (one set for each row) of NPR points tightly packed into Ceil( NPR/8 ) Connectivity Cards (format C), for a total of NPS × Ceil( NPR/8 ) cards. Cards C Variable 1 N1 Type I 2 N2 I 3 N3 I 4 N4 I 5 N5 I 6 N6 I 7 N7 I 8 N8 I Default none none none none none none none none Weight cards. Additional cards for WFL ≠ 0. Set a weight for each control point. These cards have an ordering identical to the Connectivity Cards (cards “C”). Cards D 1 Variable W1 2 W2 3 W3 4 W4 5 W5 6 W6 7 W7 8 W8 Type F F F F F F F F Default none none none none none none none none Trimming Loop cards. Additional cards for NL.gt.0. For every trimming loop (NL) define a set of Cards (E1 and E2). Cards E1 1 2 3 4 5 6 7 8 Variable NLE Type I Trimming Loop cards. Define NLE (Number of loop edges) edges (Ei). Use as many cards (E2) as necessary Cards E2 Variable 1 E1 Type I 2 E2 I 3 E3 I 4 E4 I 5 E5 I 6 E6 I 7 E7 I 8 E8 I VARIABLE DESCRIPTION NPID Nurbs-Patch Element ID. A unique number has to be chosen PID NPR PR Part ID, see *PART. Number of control points in local r-direction. Order of polynomial of univariate nurbs basis functions in local r-direction. NPS PS Number of control points in local s-direction. Order of polynomial of univariate nurbs basis functions in local s-direction. WFL Flag for weighting factors of the control points EQ.0: all weights at the control points are set to 1.0 (B-spline basis) and no optional cards D are allowed NE.0: the weights at the control points are defined in optional cards D which must be defined after cards C. FORM Shell formulation to be used EQ.0: EQ.1: shear deformable shell theory with rotational DOFs shear deformable shell theory without rotational DOFs EQ.2: thin shell theory without rotational DOFs EQ.-4/4: combination of FORM = 0 and FORM = 1 INT In-plane numerical integration rule. EQ.0: uniformly reduced Gauss integration, NIP = PR × PS. EQ.1: full Gauss integration, NIP = (PR+1) × (PS+1). EQ.2: reduced, patch-wise integration rule for C1-continuous quadratic NURBS NISR NISS Number of (automatically created) Interpolation Shell elements in local r-direction per created Nurbs-element for visualization (postprocessing) and contact . Number of (automatically created) Interpolation Shell elements in local s-direction per created Nurbs-element for visualization (postprocessing) and contact . IMASS Option for lumping of mass matrix: EQ.0: row sum EQ.1: diagonal weighting. NL Number of trimming loops EQ.0: no trimming loops – standard untrimmed NURBS GT.0: trimmed NURBS with NL trimming loops Values of the univariate knot vector in local r-direction defined in cards A. Values of the univariate knot vector in local s-direction defined in cards B. Control points i (defined via *NODE) to define the control grid in cards C. LT.0 (FORM = 4/-4): control point with rotational DOFs (6 DOFs/control point, see remark 3) Weighting factors of the control point i defined in cards D. Number of loop edges to define trimming loop in cards E1 (NL.gt.0) Edge (Curve) ID defining this edge – use *DEFINE_CURVE with DATTYP = 6 RKi SKi Ni Wi NLE Ei Remarks: 1. The thickness of the shell is defined in *SECTION_SHELL (referenced via *PART). 2. ELFORM = 201 has to be used in *SECTION_SHELL. 3. FORM = 4 allows the mixture of control points with and without rotational DOFs. This might be useful at the boundaries of Nurbs-patches where the continuity usually drops to C0 and rotational DOFs are necessary. To indicate control points with rotational DOFs (6 DOFs/control point), the node number of the corresponding control point has to be set as the negative node ID in the connectivity cards C. Positive node IDs indicate control points without rota- tional DOFs (3 DOFs/control point). If FORM = -4 is used, the control points at the patch boundary are automatically treated with rotational DOFs without the need to specify them explicitly in the connectivity cards C. This might be sufficient in many cases. 4. The post-processing and the treatment of contact boundary conditions are presently dealt with interpolation elements, defined via interpolation nodes. These nodes and elements are automatically created, where NISR and NISS indicate the number of interpolation elements to be created per NURBS-element in the local r- and s-direction, respectively . individual edges 5. Trimmed NURBS-patches can be analyzed by defining trimming loops (NL.gt.0) in Card 2. For each trimming loop to be defined, a set of cards E (E1 and E2), specifying the number of edges together with the edge (curve) IDs of is defined via the *DEFINE_CURVE using DATTYP = 6. The order of the edges as well as the order of the vertex nodes in *DEFINE_CURVE need to be in order, to define either a clockwise or a counter-clockwise orientation of the trimming loop. The orientation of the trimming loop is essential in defining, which part of the patch shall be trimmed away. Travelling along the trimming loop, the right-hand side of the trimming line will be cut away. is necessary. One edge itself 6. The trimming loops need to be defined in the parametric (local) rs-space of the NURBS-patch with r/s in [0,1]. The last and the first vertex node of consecutive edges need to coincide. Nurbs-Surface (physical space) 38 37 36 27 26 39 28 29 35 25 17 16 18 19 34 24 15 23 14 33 32 31 22 13 21 12 11 Nurbs-Surface (parameter space) - ) - ( ] , , , , , , [ : - B-spline basis functions (r-direction) r-knot: [0,0,0,1,2,3,4,5,6,7,7,7] Control Points (*NODE) Control Net (*ELEMENT_SHELL_NURBS_PATCH) Connectivity of Nurbs-Element (automatic) Nurbs-Element (automatic) Interpolation Node (automatic) Interpolation Element (automatic) Interpolation Elements (postprocessing/contact/BC) NISR=2 / NISS=2 Figure 17-27. Illustration of example input deck from Figure 17-28. *ELEMENT_SHELL_NURBS_PATCH $ Card 1 $---+-NPID----+--PID----+--NPR----+---PR----+--NPS----+---PS----+----7----+----8 2 11 12 4 9 $ Card 2 $---+--WFL----+-FORM----+--INT----+-NISR----+-NISS----+IMASS----+----7----+----8 2 1 0 1 2 $ Cards A $rk-+----1----+----2----+----3----+----4----+----5----+----6----+----7----+----8 5.0 2.0 3.0 4.0 0.0 6.0 0.0 7.0 0.0 7.0 1.0 7.0 $ Cards B $sk-+----1----+----2----+----3----+----4----+----5----+----6----+----7----+----8 0.0 0.0 0.0 1.0 2.0 2.0 2.0 $ Cards C $net+---N1----+---N2----+---N3----+---N4----+---N5----+---N6----+---N7----+---N8 4 7 3 5 2 6 12 22 32 13 23 33 14 24 34 15 25 35 16 26 36 17 27 37 18 28 38 $ Cards D (optional if WFL.ne.0) $wgt+---W1----+---W2----+---W3----+---W4----+---W5----+---W6----+---W7----+---W8 0.8 0.7 0.8 0.9 0.8 0.9 0.7 0.7 0.6 0.9 0.6 0.5 0.8 0.5 0.4 0.7 0.6 0.5 0.8 0.7 0.6 0.9 0.6 0.5 0.7 0.7 0.6 0.8 1 11 19 21 29 31 39 1.0 1.0 0.8 0.8 0.7 0.7 1.0 1.0 Figure 17-28. Example of a bi-quadratic *ELEMENT_SHELL_NURBS_- PATCH keyword definition. See Figure 17-27 below. *ELEMENT_SHELL_SOURCE_SINK Purpose: Define a strip of shell elements of a single part ID to simulate a continuous forming operation. This option requires logical regular meshing of rectangular elements, which implies that the number of nodal points across the strip is constant along the length. Elements are created at the source and disappear at the sink. The advantage of this approach is that it is not necessary to define an enormous number of elements to simulate a continuous forming operation. Currently, only one source-sink definition is allowed. The boundary conditions at the source are discrete nodal point forces to keep the work piece in tension. At the sink, displacement boundary conditions are applied. Card 1 2 3 4 5 6 7 8 Variable NSSR NSSK PID Type I I I Default none none none VARIABLE DESCRIPTION NSSR NSSK Node set at source. Provide an ordered set of nodes between corner nodes, which include the corner nodes. Node set at sink. Provide an ordered set of nodes between corner nodes, which include the corner nodes. PID Part ID of work piece. *ELEMENT_SOLID_{OPTION} Available options include: <BLANK> ORTHO DOF TET4TOTET10 H20 H8TOH20 H27 H8TOH27 Purpose: Define three-dimensional solid elements including 4 noded tetrahedrons and 8-noded hexahedrons. The type of solid element and its formulation is specified through the part ID and the section ID . Also, a local coordinate system for orthotropic and anisotropic materials can be defined by using the ORTHO option. If extra degrees of freedom are needed, the DOF option should be used. The option TET4TOTET10 converts 4 node tetrahedrons to 10 node tetrahedrons, and H8TOH20/H8TOH27 converts 8-node hexahedrons to 20-node/27- node hexahedrons. See Remark 1. Card 1 1 2 3 4 5 6 7 8 9 10 Variable EID PID Type I I Default none none Remarks Card 2 1 2 3 4 5 6 7 8 9 10 Variable N1 N2 N3 N4 N5 N6 N7 N8 N9 N10 Type I I I I I I I I I I Default none none none none none none none none none none 20 Node Element Card. Additional card for the 20 option. Card 3 1 2 3 4 5 6 7 8 9 10 Variable N11 N12 N13 N14 N15 N16 N17 N18 N19 N20 Type I I I I I I I I I I Default none none none none none none none none none none 27 Node Element Card. Additional card for the 27 option. Card 3 1 2 3 4 5 6 7 8 9 10 Variable N11 N12 N13 N14 N15 N16 N17 N18 N19 N20 Type I I I I I I I I I I Default none none none none none none none none none none Variable N21 N22 N23 N24 N25 N26 N27 Type I I I I I I I Default none none none none none none none Orthotropic Card 1. Additional card for ORTHO keyword option. Card 4 1 2 3 4 5 6 7 8 9 10 Variable A1 or BETA Type Default F 0. Remarks 5, 7 A2 F 0. A3 F 0. Orthotropic Card 2. Second additional card for ORTHO keyword option. Card 5 1 2 3 4 5 6 7 8 9 10 Variable D1 Type Default Remarks F 0. 5 D2 F 0. D3 F 0. Scalar Node Card. Additional cards for DOF keyword option. This input ends at the next keyword “*” card. Card 6 1 2 3 4 5 6 7 8 9 10 Variable NS1 NS2 NS3 NS4 NS5 NS6 NS7 NS8 Type I I I I I I I I Default none none none none none none none none VARIABLE DESCRIPTION EID Element ID. A unique number has to be chosen. VARIABLE DESCRIPTION PID Part ID, see *PART. N1 N2 N3 ⋮ Nodal point 1 Nodal point 2 Nodal point 3 ⋮ N27 Nodal point 27 A1 or BETA 𝑥-component of local material direction a, or else rotation angle BETA in degrees . 10 15 16 20 17 14 19 18 13 11 12 10 4-node n1, n2, n3, n4, n4, n4, n4, n4 6-node n1, n2, n3, n4, n5, n5, n6 ,n6 Figure 17-29. Four, six, eight, ten, and twenty node solid elements. For the hexahedral and pentahedral shapes, nodes 1-4 are on the bottom surface. VARIABLE DESCRIPTION A2 A3 D1 D2 𝑦-component of local material direction 𝐚. 𝑧-component of local material direction 𝐚. 𝑥-component of vector in the plane of the material vectors 𝐚 and 𝐛. 𝑦-component of vector in the plane of the material vectors 𝐚 and 𝐛. VARIABLE DESCRIPTION 𝑧-component of vector in the plane of the material vectors 𝐚 and 𝐛. Scalar node 1. See Remark 8. Scalar node 2 Scalar node 3 Scalar node 4 Scalar node 5 Scalar node 6 Scalar node 7 Scalar node 8 D3 NS1 NS2 NS3 NS4 NS5 NS6 NS7 NS8 Remarks: 1. Automatic Node Generation. The option TET4TOTET10 automatically converts 4 node tetrahedron solids to 10 node quadratic tetrahedron solids. Additional mid-side nodes are created which are shared by all tetrahedron elements that contain the edge. The user node ID’s for these generated nodes are offset after the largest user node ID defined in the input file. When defining the *SECTION_SOLID keyword, the element type must be specified as either 16 or 17 which are the 10-noded tetrahedrons in LS-DYNA. Mid-side nodes creat- ed as a result of TET4TOTET10 will not be automatically added to node sets that include the nodes of the original tetrahedron. So, for example, if the tetra- hedrons are to have an initial velocity, velocity initialization by part ID or part set ID using *INITIAL_VELOCITY_GENERATION is necessary as opposed to velocity initialization by node set ID using *INITIAL_VELOCITY. The option H8TOH20/H8TOH27 provides the same functionality for converting 8-node to 20-node/27-node elements. 2. Node Numbering. Four, six, and eight node elements are shown in Figure 17-29 where the ordering of the nodal points is shown. 27-node elements are shown in Figure 0-3. This ordering must be followed or code termination with occur during the initialization phase with a negative volume message. The input of nodes on the element cards for the tetrahedron and pentahedron ele- ments is given by: 4-noded tetrahedron N1, N2, N3, N4, N4, N4, N4, N4, 0, 0 c is orthogonal to the a,d plane c = a × d a,d are input. The computed axes do not depend on the element. b = c × a b is orthogonal to the c,a plane Figure 17-30. Two vectors a and d are defined and the triad is computed and stored. 6-noded pentahedron N1, N2, N3, N4, N5, N5, N6, N6, 0, 0 3. Degenerate Solids. If hexahedrons are mixed with tetrahedrons and pentahedrons in the input under the same part ID, degenerate tetrahedrons and pentahedrons are used. One problem with degenerate elements is related to an uneven mass distribution (node 4 of the tetrahedron has five times the mass of nodes 1-3) which can make these elements somewhat unstable with the default time step size. By using the control flag under the keyword, *CONTROL_SOL- ID, automatic sorting can be invoked to treat the degenerate elements as type 10 and type 15 tetrahedron and pentahedron elements, respectively. 4. Obsolete Card Format. For elements with 4-8 nodes the cards in the format of LS-DYNA versions 940-970 are still supported. The older format does not in- clude Card 2. Obsolete Element Solid Card. Card 1 1 2 3 4 5 6 7 8 9 Variable EID PID N1 N2 N3 N4 N5 N6 N7 10 N8 Type I I I I I I I I I I 5. Local Directions. For the orthotropic and anisotropic material models the local directions may be defined on the second card following the element con- nectivity definition. The local directions are then computed from the two vec- tors such that : 𝐜 = 𝐚 × 𝐝 and 𝐛 = 𝐜 × 𝐚. These vectors are internally normalized within LS-DYNA. If the material mod- el uses AOPT = 3, the 𝑎 and 𝑏 axes will be rotated about the 𝑐 axis by the BETA angle on the material card. 6. Stress Output Coordinates. Stress output for solid elements is in the global coordinate system by default. 7. Interpretation of A1 Field. If vector 𝐝 is input as a zero length vector, then A1 is interpreted as an offset rotation angle BETA in degrees which describes a rotation about the 𝐜-axis of the 𝐚-𝐛-𝐜 coordinate system that is defined by AOPT and associated parameters on the *MAT input. This BETA angle applies to all values of AOPT, and it overrides the BETA angle on the *MAT card in the case of AOPT=3. 7 14 15 8. Optional “Scalar” Nodes. The scalar nodes specified on the optional card refer to extra nodes used by certain features (usual user defined) to store addi- tional degrees of freedom. 16 26 8 13 17 18 19 3 10 11 12 0 4 22 23 24 27 21 25 Figure 17-3. 27-node solid element. *ELEMENT_SOLID_NURBS_PATCH Purpose: Define a NURBS-block element (patch) based on a cuboid grid of control points. This grid consists of NPR*NPS*NPT control points, where NPR, NPS and NPT are the number of control points in local r-, s- and t-direction, respectively. The necessary shape functions are defined through three knot-vectors: 1. Knot-Vector in r-direction with length NPR + PR + 1 and 2. Knot-Vector in s-direction with length NPS + PS + 1 and 3. Knot-Vector in t-direction with length NPT + PT + 1 and There is no limit on the size of the underlying grid to define a NURBS-block element, so the total number of necessary Keyword-cards depends on the parameters given in the first two cards and is given by # of cards = 2 + ⌈ NPR + PR + 1 ⌉ + ⌈ NPS + PS + 1 ⌉ + ⌈ NPT + PT + 1 ⌉ + NPT × NPS × ⌈ NPR ⌉, where ⌈𝑥⌉ = ceil(𝑥). (NOTE: the last term in the sum is doubled if WFL = 1, indicating that the weights are user-specified). An example partial keyword deck using this card is given at the end. Card 1 1 2 3 Variable NPID PID NPR Type I I I 4 PR I 5 NPS I 6 PS I 7 NPT I 8 PT I Default none none none none none none none none Card 2 1 2 3 4 5 6 7 8 Variable WFL NISR NISS NIST IMASS Type Default I 0 Remarks I I I PR PS PT I 0 Knott Vector Cards (for r-direction). The knot-vector in local r-direction with length NPR +PR + 1 is given below (up to eight values per card) requiring a total of Ceil[ (NPR +PR + 1)/8 ] cards. Cards A 1 2 3 4 5 6 7 8 Variable RK1 RK2 RK3 RK4 RK5 RK6 RK7 RK8 Type F F F F F F F F Default none none none none none none none none Knott Vector Cards (for s-direction). The knot-vector in local s-direction with length NPS +PS + 1 is given below (up to eight values per card) requiring a total of Ceil[ (NPS +PS + 1)/8 ] cards. Cards B 1 2 3 4 5 6 7 8 Variable SK1 SK2 SK3 SK4 SK5 SK6 SK7 SK8 Type F F F F F F F F Default none none none none none none none none Knott Vector Cards (for t-direction). The knot-vector in local t-direction with length NPT +PT + 1 is given below (up to eight values per card) requiring a total of Ceil[ (NPT+PT + 1)/8 ] cards. Cards C 1 2 3 4 5 6 7 8 Variable TK1 TK2 TK3 TK4 TK5 TK6 TK7 TK8 Type F F F F F F F F Default none none none none none none none none Connectivity Cards. The connectivity of the control grid is a two dimensional table of NPT × NPS rows and NPR columns. This data fills NPT × NPS sets (one set for each row) of NPR points tightly packed into Ceil( NPR/8 ) Connectivity Cards (format C), for a total of NPT × NPS × Ceil( NPR/8 ) cards. Cards D Variable 1 N1 Type I 2 N2 I 3 N3 I 4 N4 I 5 N5 I 6 N6 I 7 N7 I 8 N8 I Default none none none none none none none none Weight cards. Additional cards for WFL ≠ 0. Set a weight for each control point. These cards have an ordering identical to the Connectivity Cards (cards “D”). Cards E 1 Variable W1 2 W2 3 W3 4 W4 5 W5 6 W6 7 W7 8 W8 Type F F F F F F F F Default none none none none none none none none VARIABLE DESCRIPTION NPID Nurbs-Patch Element ID. A unique number has to be chosen PID NPR PR NPS PS NPT PT Part ID, see *PART. Number of control points in local r-direction. Order of polynomial of univariate nurbs basis functions in local r-direction. Number of control points in local s-direction. Order of polynomial of univariate nurbs basis functions in local s-direction. Number of control points in local t-direction. Order of polynomial of univariate nurbs basis functions in local t-direction. WFL Flag for weighting factors of the control points EQ.0: all weights at the control points are set to 1.0 (B-spline basis) and no optional cards E are allowed NE.0: the weights at the control points are defined in optional cards E which must be defined after cards D. Number of (automatically created) Interpolation Solid elements in local r-direction per created Nurbs-element for visualization (postprocessing) and contact. Number of (automatically created) Interpolation Solid elements in local s-direction per created Nurbs-element for visualization (postprocessing) and contact. Number of (automatically created) Interpolation Solid elements in local t-direction per created Nurbs-element for visualization (postprocessing) and contact. NISR NISS NIST IMASS Option for lumping of mass matrix: EQ.0: row sum EQ.1: diagonal weighting. RKi SKi Values of the univariate knot vector in local r-direction defined in cards A. Values of the univariate knot vector in local s-direction defined in cards B. Values of the univariate knot vector in local t-direction defined in cards C. Control points i (defined via *NODE) to define the control grid in cards D. Weighting factors of the control point i defined in cards E. TKi Ni Wi Remarks: 1. ELFORM = 201 has to be used in *SECTION_SOLD. 2. The post-processing and the treatment of contact boundary conditions are presently dealt with interpolation elements, defined via interpolation nodes. These nodes and elements are automatically created, where NISR, NISS and NIST indicate the number of interpolation elements to be created per NURBS- element in the local r-, s- and t-direction, respectively. 3. An input deck can be shown as follows. Example: $...|....1....|....2....|....3....|....4....|....5....|....6....|....7....|....8 $ An Isogeometric Solid NURBS Example : $...|....1....|....2....|....3....|....4....|....5....|....6....|....7....|....8 *SECTION_SOLID $# secid elform 1 201 *ELEMENT_SOLID_NURBS_PATCH $CARD 1 $# npeid pid npr pr nps ps npt pt 1 1 3 2 6 2 3 2 $CARD 2 $# wfl nisr niss nist imass 0 2 2 2 0 $CARD A $# rk1 rk2 rk3 rk4 rk5 rk6 rk7 rk8 0.0 0.0 0.0 1.0 1.0 1.0 $CARD B 0.0 0.0 0.0 0.25 0.5 0.75 1.0 1.0 1.0 $CARD C 0.0 0.0 0.0 1.0 1.0 1.0 $CARD D 1001 1002 1003 … 1052 1053 1054 $CARD E (Optional if wfl .eq. 0) *ELEMENT_SPH Purpose: Define a lumped mass element assigned to a nodal point. Card 1 2 3 4 5 6 7 8 9 10 Variable NID PID MASS Type I I Default none none Remarks F 0. 1 VARIABLE DESCRIPTION Node ID and Element ID are the same for the SPH option. Part ID to which this node (element) belongs. GT.0: Mass value LT.0: Volume. The absolute value will be used as volume. The density (rho) will be retrieved from the material card defined in PID. SPH element mass is calculated by abs(MASS) × ρ. NID PID MASS Remarks: 1. Axisymmetric SPH, IDIM = -2 in CONTROL_SPH, is defined on global X-Y plane, with Y-axis as the axis of rotation. An axisymmetric SPH element has a mass of Aρ, where ρ is its density, A is the area of the SPH element and can be approximated by the area of its corresponding axisymmetric shell element, Fig. 1. The mass printout in d3hsp is the mass per radian, i.e., Aρxi, Fig. 1 & 2. Y xi A,ρ X 1 rad xi Aρ X Axisymmetric SPH / corresponding shell Mass printout in d3hsp, mass/radian Mass printout in d3hsp, mass/radian *ELEMENT_TRIM NOTE: This keyword was replaced by *CONTROL_FORM- ING_TRIMING starting in Revision 87566. *ELEMENT_TSHELL_{OPTION} Available options include: <BLANK> BETA COMPOSITE Purpose: Define an eight node thick shell element which is available with either fully reduced or selectively reduced integration rules. Thick shell formulations 1, 2, and 6 are plane stress elements that can be used as an alternative to the 4 node shell elements in cases where an 8-node element is desired. Thick shell formulations 3, 5 and 7 are layered solids with 3D stress updates. Formulation 5, 6, and 7 are based on an enhanced strain. The number of through-thickness integration points is specified by the user. For orthotropic and anisotropic materials, a local material angle (variable BETA) can be defined which is cumulative with the integration point angles specified in *SECTION_- TSHELL or *PART_COMPOSITE_TSHELL. The COMPOSITE option for *ELEMENT_TSHELL allows a unique stackup of integration points for each element sharing the same part ID, and is available only when combined with *PART. The COMPOSITE option is not available in combination with *PART_COMPOSITE_TSHELL. To maintain a direct association of through-thickness integration point numbers with physical plies in the case where the number of plies varies from element to element, see Remark 5. Card 1 1 2 3 4 5 6 7 8 9 Variable EID PID N1 N2 N3 N4 N5 N6 N7 10 N8 Type I I I I I I I I I I Default none none none none none none none none none none Remarks Beta Card. Additional card for BETA keyword option. Card 2 1 2 3 4 5 6 7 8 9 10 Variable Type Default Remarks BETA F 0. 4 Composite Card. Additional card for COMPOSITE keyword option. The material ID, thickness, and material angle for each through-thickness integration point of a composite shell are defined. The integration point data should be given sequentially starting with the bottommost integration point. The total number of integration points is determined by the number of entries on these cards. The total thickness is the distance between the top and bottom surface as determined by the element connectivity, so the THICKi values are scaled to fit the element. Define as many cards as needed. The input ends at the next keyword (“*”) card. Card 2 1 2 Variable MID1 THICK1 Type I Card 2 1 F 2 Variable MID3 THICK3 Type I F 3 B1 F 3 B3 F 4 5 6 MID2 THICK2 F 6 I 5 Etc. 4 7 B2 F 7 I F F 8 8 VARIABLE DESCRIPTION EID PID N1 Element ID. Unique numbers have to be used. Part ID, see *PART. Nodal point 1 n5 n1 n8 n4 n6 n2 n7 n3 Figure 17-31. 8-node Thick Shell Element. VARIABLE DESCRIPTION N2 N3 ⋮ N8 BETA Nodal point 2 Nodal point 3 ⋮ Nodal point 8 Orthotropic material base offset angle . The angle is given in degrees. If blank the default is set to zero. MIDi Material ID of integration point i, see the *MAT_… cards. THICKi Thickness of integration point i Bi Material angle of integration point i Remarks: 1. Orientation. Extreme care must be used in defining the connectivity to ensure proper orientation of the through-thickness direction. For a hexahedron, nodes 𝑛1 to 𝑛4 define the lower surface, and nodes 𝑛5 to 𝑛8 define the upper surface. For a pentahedron, nodes 𝑛1, 𝑛2, 𝑛3 form the lower triangular surface and the eight variables N1 to N8 should be defined using nodes 𝑛1, 𝑛2, 𝑛3, 𝑛3, 𝑛4, 𝑛5, 𝑛6, 𝑛6, respectively. Note that node 𝑛3 and node 𝑛6 are each repeated. 2. Integration. Element formulations 1 and 5 , use one point integration and the integration points then lie along the 𝑡-axis as shown in Figure 17-31. Element forumulations 2 and 3 use two by two selective reduced integration in each layer. 3. Stress Output. The stresses for thick shell elements are output in the global coordinate system. 4. Local Coordinate System. To allow the orientation of orthotropic and anisotropic materials to be defined for each thick shell element, a beta angle can be defined. This beta angle is used with the AOPT parameter and associated data on the *MAT card to determine an element reference direction for the element. The AOPT data defines a coordinate system and the BETA angle defines a sub- sequent rotation about the element normal to determine the element reference system. For composite modeling, each layer in the element can have a unique material direction by defining an additional rotation angle for the layer, using either the ICOMP and Bi parameters on *SECTION_TSHELL or the Bi parame- ter on *PART_COMPOSITE_TSHELL. The material direction for layer i is then determined by a rotation angle, 𝜃𝑖. 5. Assignment of Zero Thickness to Integration Points. The ability to assign zero- thickness integration points in the stacking sequence allows the number of integration points to remain constant even as the number of physical plies var- ies from element to element and eases post-processing since a particular inte- gration point corresponds to a physical ply. Such a capability is important when one or more of the physical plies are not continuous across a part. To represent a missing ply in *ELEMENT_TSHELL_COMPOSITE, set THICKi to 0.0 for the corresponding integration point and additionally, set MID to -1. When postprocessing the results using LS-PrePost version 4.5, read both the keyword deck and d3plot database into the code and then select Option > N/A gray fringe. Then, when viewing fringe plots for a particular integration point (FriComp > IPt > intpt#), the element will be grayed out if the selected integra- tion point is missing (or has zero thickness) in that element. *END The *END command is optional and signals the conclusion of a keyword input file. Data in a keyword file beyond a *END command are not read by LS-DYNA. Please see LS-DYNA Keyword User’s Manual, Volume II (Material Models). Purpose: The keyword *FREQUENCY_DOMAIN provides a way of defining and solving frequency domain vibration and acoustic problems. The keyword cards in this section are defined in alphabetical order: *FREQUENCY_DOMAIN_ACCELERATION_UNIT *FREQUENCY_DOMAIN_ACOUSTIC_BEM_{OPTION} *FREQUENCY_DOMAIN_ACOUSTIC_FEM *FREQUENCY_DOMAIN_ACOUSTIC_FRINGE_PLOT_{OPTION} *FREQUENCY_DOMAIN_ACOUSTIC_INCIDENT_WAVE *FREQUENCY_DOMAIN_ACOUSTIC_SOUND_SPEED *FREQUENCY_DOMAIN_FRF *FREQUENCY_DOMAIN_MODE_{OPTION} *FREQUENCY_DOMAIN_PATH *FREQUENCY_DOMAIN_RANDOM_VIBRATION_{OPTION} *FREQUENCY_DOMAIN_RESPONSE_SPECTRUM *FREQUENCY_DOMAIN_SSD *FREQUENCY_DOMAIN_ACCELERATION_UNIT Purpose: LS-DYNA’s default behavior is to assume that accelerations are derived: [acceleration unit] = [length unit] [time unit]2 . This card extends LS-DYNA to support other units for acceleration. Card 1 1 2 Variable UNIT UMLT Type I F VARIABLE DESCRIPTION UNIT Flag for acceleration unit conversion: EQ.0: use [length unit]/[time unit]2 as unit of acceleration. EQ.1: use 𝑔 as unit for acceleration, and SI units (Newton, kg, meter, second, etc.) elsewhere. EQ.2: use 𝑔 as unit for acceleration, and Engineering units (lbf, lbf × second2/inch, inch, second, etc.) elsewhere. EQ.3: use 𝑔 as unit for acceleration, and units (kN, kg, mm, ms, GPa, etc.) elsewhere. EQ.-1: use 𝑔 as unit for acceleration and provide the multiplier for converting g to [length unit]/[time unit]2. UMLT Multiplier for converting 𝑔 to [length unit]/[time unit]2 (used only for UNIT = -1). Remarks: LS-DYNA uses consistent units. With consistent units acceleration is defined using: [acceleration unit] = [length unit] [time unit]2 . However, it is the convention of many industries to use 𝑔 (gravitational acceleration on the Earth’s surface) as the base unit for acceleration. Usually, data from vibration tests, both random and sine sweep, are expressed in systems for which 𝑔 is the unit of acceleration. With this keyword, LS-DYNA supports such conventions. Internally, LS- DYNA implements this keyword by converting the input deck into consistent units, and then proceeding with the calculation as usual. However, results are output in the unit system specified with this keyword. *FREQUENCY_DOMAIN_ACOUSTIC_BEM_{OPTION1}_{OPTION2} Available options include: ATV MATV HALF_SPACE PANEL_CONTRIBUTION Purpose: Activate the boundary element method in frequency domain for acoustic problems. This keyword is ignored unless the BEM=filename option is included in the LS-DYNA command line: Control Card. To use this card LS-DYNA must be run with a BEM option, as in “LS- DYNA I=inf BEM=filename”. 3 4 5 6 7 8 FMIN FMAX NFREQ DTOUT TSTART PREF Card 1 Variable 1 RO Type F 2 C F F F I 0 F 0 Default none none none none Remark F 0 1 7 F 0 2 8 Card 2 1 2 3 4 5 6 Variable NSIDEXT TYPEXT NSIDINT TYPINT FFTWIN TRSLT IPFILE IUNITS I 0 I 0 I 0 I 0 Type Default Remark I 0 I 0 3 I 0 4 I 0 Additional card for FFTWIN = 5. Card 2a 1 2 3 4 5 6 7 8 Variable T_HOLD DECAY Type F F Default 0.0 0.02 Card 3 1 2 3 4 5 6 7 8 Variable METHOD MAXIT TOLITR NDD TOLLR TOLFCT IBDIM NPG Type I I F Default 100 10-4 Remark 6 Card 4 1 2 3 I 1 7 4 F F I 10-6 10-6 1000 I 2 5 6 7 8 Variable NBC RESTRT IEDGE NOEL NFRUP VELOUT DBA Type Default Remark I 1 I 0 8 I 0 9 I 0 I 0 I 0 I 0 10 11 Boundary Condition Cards. The deck must include NBC cards in this format: one for each boundary condition. Card 5 1 2 3 4 5 6 7 8 Variable SSID SSTYPE NORM BEMTYP LC1 LC2 Type Default I 0 I 0 I 0 I 0 I I Remark 12 Panel Contribution Card. Additional for PANEL_CONTRIBUTION keyword option. Card 6 1 2 3 4 5 6 7 8 Variable NSIDPC Type Default I 0 Remark 13 Half Space Card. Additional card for HALF_SPACE keyword option. Card 6 1 2 3 4 5 6 7 8 Variable PID Type Default I 0 VARIABLE DESCRIPTION RO Fluid density. VARIABLE DESCRIPTION C Sound speed of the fluid. GT.0: real constant sound speed. LT.0: |C| is the load curve ID, which defines the frequency dependent complex sound speed. See *FREQUENCY_- DOMAIN_ACOUSTIC_SOUND_SPEED. FMIN FMAX Minimum value of output frequencies. Maximum value of output frequencies. NFREQ Number of output frequencies. DTOUT TSTART PREF Time interval between writing velocity or acceleration, and pressure at boundary elements in the binary file, to be proceeded at the end of LS-DYNA simulation. Start time for recording velocity or acceleration in LS-DYNA simulation. Reference pressure to be used to output pressure in dB, in the file Press_dB. If PREF = 0, the Press_dB file will not be generated. A file called Press_Pa is generated and contains the pressure at the output nodes . NSIDEXT Node or segment set ID of output exterior field points. TYPEXT Output exterior field point type. EQ.0: node ID. EQ.1: node set ID. EQ.2: segment set ID. NSIDINT Node or segment set ID of output interior field points. TYPINT Output interior field point type. EQ.0: node ID. EQ.1: node set ID. EQ.2: segment set ID. VARIABLE DESCRIPTION FFTWIN FFT windows (Default = 0). EQ.0: rectangular window. EQ.1: Hanning window. EQ.2: Hamming window. EQ.3: Blackman window. EQ.4: raised cosine window. EQ.5: exponential window. TRSLT Request time domain results: EQ.0: no time domain results are requested. EQ.1: time domain results are requested (Press_Pa_t gives absolute value pressure vs. time). EQ.2: time domain results are requested (Press_Pa_t gives real value pressure vs. time). VARIABLE DESCRIPTION IPFILE Flag for output files (default = 0): EQ.0: Press_Pa (magnitude of pressure vs. frequency), Press_dB (sound pressure level vs. frequency) and bepres (ASCII database file for LS-Prepost) are provid- ed. EQ.1: Press_Pa_real (the real part of the pressure vs. frequency) and Press_Pa_imag (the imaginary part of the pressure vs. frequency) are provided, in addition to Press_Pa, Press_dB and bepres. EQ.10: files for IPFILE = 0, and fringe files for acoustic pressure. EQ.11: files for IPFILE = 1, and fringe files for acoustic pressure. EQ.20: files for IPFILE = 0, and fringe files for sound pressure level. EQ.21: files for IPFILE = 1, and fringe files for sound pressure level. EQ.31: files for IPFILE = 1, and fringe files for acoustic pressure (real part). EQ.41: files for IPFILE = 1, and fringe files for acoustic pressure (imaginary part). IUNITS Flag for unit changes EQ.0: do not apply unit change. EQ.1: MKS units are used, no change needed. EQ.2: units: lbf × s2/in, inch, s, lbf, psi, etc. are used, changed to MKS in BEM Acoustic computation. EQ.3: units: kg, mm, ms, kN, GPa, etc. are used, changed to MKS in BEM acoustic computation. EQ.4: units: ton, mm, s, N, MPa, etc. are used, changed to MKS in BEM acoustic computation. T_HOLD Hold-off period before the exponential window. The length of the hold-off period should coincide with the pre-trigger time to reduce the effects of noise in the captured time domain data. It is only used when FFTWIN = 5. VARIABLE DECAY DESCRIPTION Decay ratio at the end of capture duration. For example, if the DECAY = 0.02, it means that the vibration is forced to decay to 2% of its amplitude within the capture duration. This field is only used when FFTWIN = 5. METHOD Method used in acoustic analysis EQ.0: Rayleigh method (very fast). EQ.1: Kirchhoff method coupled to FEM for acoustics (*MAT_- ACOUSTIC). See Remark 6. EQ.2: variational Indirect BEM. EQ.3: collocation BEM. EQ.4: collocation BEM with Burton-Miller formulation for exterior problems (no irregular frequency phenomenon). MAXIT Maximum number of iterations for iterative solver (default = 100) if METHOD ≥ 2. TOLITR Tolerance for the iterative solver. The default value is 10−4. NDD Number of domain decomposition, used for memory saving. For large problems, the boundary mesh is decomposed into NDD domains for less memory allocation. This option is only used if METHOD ≥ 2. TOLLR Tolerance for (default = 10−6). low rank approximation of dense matrix TOLFCT Tolerance in factorization of the low rank matrix (default = 10−6). IBDIM Inner iteration limit in GMRES iterative solver (default = 1000). NPG NBC RESTRT Number of Gauss integration points (default = 2). Number of boundary condition cards. See Card 5. (default = 1). This flag is used to save an LS-DYNA analysis if the binary output file in the (bem=filename) option has not been changed (default = 0). EQ.0: LS-DYNA time domain analysis generates a new binary file. is processed and EQ.1: LS-DYNA time domain analysis is not processed. The VARIABLE DESCRIPTION binary files from previous run are used. The files include the binary output file filename, and the binary file bin_velfreq, which saves the boundary velocity from FFT. EQ.2: LS-DYNA restarts from d3dump file by using “R=” command line parameter. This is useful when the last run was interrupted by sense switches such as “sw1”. EQ.3: LS-DYNA reads in user provided velocity history saved in an ASCII file, bevel. EQ.4: run acoustic computation on a boundary element mesh with velocity information given with a denser finite ele- ment mesh in last run. This option requires both “bem = filename” and “lbem = filename2” in the com- mand line, where filename2 is the name of the binary file generated in the last run with denser mesh. EQ.5: LS-DYNA time domain analysis is not processed. The binary file filename from previous run is used. An FFT is performed to get the new frequency domain boundary velocity and the results are saved in bin_velfreq. IEDGE Free edge and multi-connection constraints option (default = 0). EQ.0: free edge and multi-connection constraints not considered. EQ.1: free edge and multi-connection constraints considered. EQ.2: only free edge constraints are considered. EQ.3: only multi-connection constraints are considered. NOEL Location where normal velocity or acceleration (default = 0). is taken EQ.0: elements or segments. EQ.1: nodes. NFRUP Preconditioner update option. EQ.0: updated at every frequency. GE.1: updated for every NFRUP frequencies. VARIABLE DESCRIPTION VELOUT Flag for writing out nodal or elemental velocity data. EQ.0: No writing out velocity data. EQ.1: write out time domain velocity data (in 𝑥, 𝑦 and 𝑧 directions). EQ.2: write out frequency domain velocity data (in normal direction). DBA Flag for writing out weighted SPL files with different weighting options. EQ.0: No writing out weighted SPL files. EQ.1: write out Press_dB(A) by using A-weighting. EQ.2: write out Press_dB(B) by using B-weighting. EQ.3: write out Press_dB(C) by using C-weighting. EQ.4: write out Press_dB(D) by using D-weighting. SSID Part, part set ID, or segment set ID of boundary elements. SSTYPE Boundary element type: EQ.0: part Set ID EQ.1: part ID EQ.2: segment set ID. NORM NORM should be set such that the normal vectors point away from the fluid. EQ.0: normal vectors are not inverted (default). EQ.1: normal vectors are inverted. VARIABLE DESCRIPTION BEMTYP Type of input boundary values in BEM analysis. EQ.0: boundary velocity will be processed in BEM analysis. EQ.1: boundary acceleration will be processed in BEM analysis. EQ.2: pressure is prescribed and the real and imaginary parts are given by LC1 and LC2. EQ.3: normal velocity is prescribed and the real and imaginary parts are given by LC1 and LC2. EQ.4: impedance is prescribed and the real and imaginary parts are given by LC1 and LC2. LT.0: normal velocity (only real part) is prescribed, through load curve n. An amplitude as a function of frequency load curve with curve ID |BEMTYP|. Load curve ID for defining real part of pressure, normal velocity or impedance. Load curve ID for defining imaginary part of pressure, normal velocity or impedance. Node set ID for the field points where panel contributions to SPL (Sound Pressure Level) are requested. Plane ID for defining the half-space problem, see keyword *DE- FINE_PLANE. LC1 LC2 NSIDPC PID Remarks: 1. TSART Field. TSTART indicates the time at which velocity or acceleration and pressure are stored in the binary file. 2. PREF Field. This reference pressure is required for the computation of the pressure in dB. Usually, in International Unit System the reference pressure is 20𝜇Pa. 3. FFT Windowing. Velocity or acceleration (pressure) is provided by LS-DYNA analysis. They are written in a binary file (bem=filename). The boundary element method is processed after the LS-DYNA analysis. An FFT algorithm is used to transform time domain data into frequency domain in order to use the boundary element method for acoustics. In order to overcome the FFT leakage problem due to the truncation of the temporal response, several windows are Figure 20-1. T-section. proposed. Windowing is used to have a periodic velocity, acceleration and pressure in order to use the FFT. 4. TRSLT Field. If time domain results are requested, FMIN is changed to 0 in the code. 5. IUNITS Field. Units are automatically converted into kg, m, s, N, and Pa so that the reference pressure will not be too small. For example, it may be as low as 20.E-15 GPa if one uses the units kg, mm, ms, kN, and GPa and this may result in truncation error in the computation, especially in single precision version. 6. METHOD Field. The Rayleigh method is an approximation suitable only for external radiation problems. It is very fast since there is no linear system to solve. The Kirchhoff method involves coupling the BEM and FEM for acoustics (*MAT_ACOUSTIC) with a Non Reflecting Boundary condition, see *BOUND- ARY_NON_REFLECTING. In this case, at least one fluid layer with non- reflecting boundary condition is merged with the vibrating structure. This additional fluid is given in *MAT_ACOUSTIC by the same density and sound speed as used in this keyword. When used appropriately both methods pro- vide a good approximation to a full BEM calculation for external problems. 7. NDD Field. BEM formulation for large and medium size problems (more than 2000 boundary elements) is memory and time consuming. In this case, user may run LS-DYNA using the memory option. In order to save memory, do- main decomposition can be used. 8. RESTRT Field. The binary file generated by a previous run can be used for the next run by using the restart option. The restart option allows the user to use the binary file generated from a previous calculation in order to run BEM. In this case, the frequency range can be changed. However, the time paraemeters should not be modified between calculations. 9. IEDGE Field. This option only applies to METHOD = 2, the Variational Indirect BEM. 10. NOEL Field. This field specified whether the element or nodal velocity (or acceleration) is taken from FEM computation. NOEL should be 0 if Kirchhoff method (METHOD = 1) is used since elemental pressure is processed in FEM. NOEL should be 0 if Burton-Miller collocation method (METHOD = 4) is used since a constant strength element formulation is adopted. In other cases, it is strongly recommended to use element velocity or acceleration (NOEL = 0) if “T- Section” appears in boundary element mesh. See Figure 20-1. 11. NFRUP Field. The preconditioner is obtained with the factorization of the influence coefficient matrix. To conserve CPU time, It can be retained for sev- eral frequencies. By default (NFRUP=0), the preconditioner is updated for every frequency. Note that in MPP version, the preconditioner is updated every NFRUP frequencies on each processor. 12. Boundary Condition Cards. The Card 5 can be defined if the boundary elements are composed of several panels. It can be defined multiple times if more than 2 panels are used. Each card 5 defines one panel. 13. NSIDPC Field. The field points where the panel contribution analysis is requested must be one of the field points for acoustic computation (it must be included in the nodes specified by the NSIDEXT or NSIDINT). The panels are defined by card 4 and card 5, etc. Each card defines one panel. 14. Element Sizing. To obtain accurate results, the element size should not be greater than 1/6 of the wave length (= 𝑐/𝑓 where 𝑐 is the wave speed and 𝑓 is the frequency). 15. Acoustic Transfer Vector. The Acoustic Transfer Vector can be obtained by including the option ATV in the keyword. It calculates acoustic pressure (and sound pressure level) at field points due to unit normal velocity of each surface node. ATV is dependent on structure model, properties of acoustic fluid as well as location of field points. When ATV option is included, the structure does not need any external excitation, and the curve IDs LC1 and LC2 are ig- nored. A binary plot database d3atv can be obtained by setting BINARY = 1 in *DATABASE_FREQUENCY_BINARY_D3ATV. 16. Modal Acoustic Transfer Vector. The Modal Acoustic Transfer Vector (MATV) is calculated when the MATV keyword option is included. The MATV option requires that the implicit eigenvalue solver be used, which is activated by keywords *CONTROL_IMPLICIT_GENERAL, and *CONTROL_IMPLIC- IT_EIGENVALUE. It calculates acoustic pressure (and sound pressure level) at field points due to vibration in the form of eigenmodes. For each excitation frequency 𝑓 , LS-DYNA generates the psedo-velocity boundary condition 2𝜋𝑖𝑓 {𝜙}𝑗, where 𝑖 = √−1 is the imaginary unit and runs acoustic computation for each field point, based on the psedo-velocity boundary conditions, to get the MATV matrices. The MATV matrices are saved in binary file “bin_bepressure” for future use. Like ATV, MATV is also only dependent on structure model, properties of acoustic fluids as well as the location of field points. 17. Output Files. The result files: Press_Pa, Press_dB, Press_Pa_real, Press_Pa_ imag, Press_Pa_t and Press_dB_t have a xyplot format that LS-PrePost can read and plot. *FREQUENCY_DOMAIN_ACOUSTIC_FEM_{OPTION} Available options include: EIGENVALUE Purpose: Define an interior acoustic problem and solve the problem with a frequency domain finite element method. When EIGENVALUE option is used, compute eigenvalues and eigenvectors of the acoustic system. Card 1 Variable 1 RO Type F 2 C F F F 3 4 5 6 7 8 FMIN FMAX NFREQ DTOUT TSTART PREF Default none none none none Card 2 1 2 3 4 Variable FFTWIN I 0 5 F 0 6 F 0 7 F 0 8 Type Default Card 3 1 I 0 2 Variable PID PTYP Type I Default none I 0 3 4 5 6 7 Boundary Condition Definition Card. It can be repeated if multiple boundary conditions are present. This card is optional when option EIGENVALUE is present. Card 4 1 2 3 4 5 6 Variable SID STYP VAD DOF LCID1 LCID2 Type I Default none I 0 I 0 I none I 0 I 0 7 SF F 1.0 8 VID I 0 Field Points Definition Card. Not used when option EIGENVALUE is present. Card 5 1 2 3 4 5 6 7 8 Variable NID NTYP IPFILE DBA Type I Default none I 0 I 0 I 0 VARIABLE DESCRIPTION RO C Fluid density. Sound speed of the fluid. GT.0: real constant sound speed. LT.0: |C| is the load curve ID, which defines the frequency dependent complex sound speed. See *FREQUENCY_- DOMAIN_ACOUSTIC_SOUND_SPEED. FMIN FMAX Minimum value of output frequencies. Maximum value of output frequencies. NFREQ Number of output frequencies. DTOUT Time step for writing velocity or acceleration in the binary file. TSTART Start time for recording velocity or acceleration in transient analysis. VARIABLE DESCRIPTION PREF Reference pressure, for converting the acoustic pressure to dB. FFTWIN FFT windows (Default = 0): EQ.0: rectangular window. EQ.1: Hanning window. EQ.2: Hamming window. EQ.3: Blackman window. EQ.4: Raised cosine window. PID PTYP Part ID, or part set ID to define the acoustic domain. Set type: EQ.0: part, see *PART. EQ.1: part set, see *SET_PART. SID Part ID, or part set ID, or segment set ID, or node set ID to define the boundary where vibration boundary condition is provided STYP Set type: EQ.0: part, see *PART. EQ.1: part set, see *SET_PART. EQ.2: segment set, see *SET_SEGMENT. EQ.3: node set, see *SET_NODE. VAD Boundary condition flag: EQ.0: velocity by steady state dynamics (SSD). EQ.1: velocity by transient analysis. EQ.2: opening (zero pressure). EQ.11: velocity by LCID1 (amplitude) and LCID2 (phase). EQ.12: velocity by LCID1 (real) and LCID2 (imaginary). EQ.21: acceleration by LCID1 (amplitude) and LCID2 (phase). EQ.22: acceleration by LCID1 (real) and LCID2 (imaginary). EQ.31: displacement by LCID1 (amplitude) and LCID2 (phase). EQ.32: displacement by LCID1 (real) and LCID2 (imaginary). VARIABLE DESCRIPTION EQ.41: impedance by LCID1 (amplitude) and LCID2 (phase). EQ.42: impedance by LCID1 (real) and LCID2 (imaginary). EQ.51: pressure by LCID1 (amplitude) and LCID2 (phase). EQ.52: pressure by LCID1 (real) and LCID2 (imaginary). DOF Applicable degrees-of-freedom: EQ.0: determined by steady state dynamics. EQ.1: 𝑥-translational degree-of-freedom, EQ.2: 𝑦-translational degree-of-freedom, EQ.3: 𝑧-translational degree-of-freedom, EQ.4: translational motion in direction given by VID, EQ.5: normal direction of the element or segment. LCID1 LCID2 SF VID NID Load curve ID to describe the amplitude (or real part) of velocity, see *DEFINE_CURVE. Load curve ID to describe the phase (or imaginary part) of velocity, see *DEFINE_CURVE. Load curve scale factor. Vector ID for DOF values of 4. Node ID, or node set ID, or segment set ID for acoustic result output. NTYP Set type: EQ.0: Node, see *NODE. EQ.1: Node set, see *SET_NODE. IPFILE Flag for output files (default = 0): EQ.0: Press_Pa (magnitude of pressure vs. frequency), Press_ dB (sound pressure level vs. frequency) are provided. EQ.1: Press_Pa_real (real part of pressure vs. frequency) and Press_Pa_imag (imaginary part of pressure vs. frequen- cy) are provided, in addition to Press_Pa, Press_dB. VARIABLE DBA DESCRIPTION Flag for writing out weighted SPL files with different weighting options. EQ.0: No writing out weighted SPL files. EQ.1: write out Press_dB(A) by using A-weighting. EQ.2: write out Press_dB(B) by using B-weighting. EQ.3: write out Press_dB(C) by using C-weighting. EQ.4: write out Press_dB(D) by using D-weighting. Remarks: 1. This command solves the interior acoustic problems which is governed by Helmholtz equation ∇2𝑝 + 𝑘2𝑝 = 0 with the boundary condition ∂𝑝 ∂𝑛⁄ = −𝑖𝜔𝜌𝑣𝑛, where, 𝑝 is the acoustic pressure; 𝑘 = 𝜔/𝑐 is the wave number; 𝜔 is the round frequency; 𝑐 is the acoustic wave speed (sound speed); 𝑖 = √−1 is the imaginary unit; 𝜌 is the mass density and 𝑣𝑛 is the normal velocity. This com- mand solves the acoustic problem in frequency domain. 2. If mass density RO is not given, the mass density of PID (the part which defines the acoustic domain), will be used 3. PREF is the reference pressure to convert the acoustic pressure to dB 𝐿𝑝 = ) Note that generally 𝑝ref = 20𝜇Pa for air. 2⁄ 10 log10(𝑝2 𝑝ref 4. If the boundary velocity is obtained from steady state dynamics (VAD = 0) using the keyword *FREQUENCY_DOMAIN_SSD, the part (PID) which de- fines the acoustic domain has to use one of the following material models, a) MAT_ELASTIC_FLUID b) MAT_NULL (and EOS_IDEAL_GAS) Since only the above material models enable implicit eigenvalue analysis. If the boundary excitation is given by load curves LCID1 and LCID2 (VAD > 0), the part (PID) which defines the acoustic domain can use any material model which is compatible with 8-node solid elements, as only the mesh of the PID will be utilized in the computation. For example, MAT_ACOUSTIC and MAT_ELAS- TIC_FLUID can be used. 5. If VAD = 0, the boundary excitation is given as velocity obtained from steady state dynamics. The other parameters in Card 3 (DOF, LCID1, LCID2, SF and VID) are ignored. 6. If a node’s vibration boundary condition is defined multiple times, only the last definition is considered. This happens usually when a node is on edge and shared by two or more PART, SET_PART, SET_NODE, or SET_SEGMENT and different vibration condition is defined on each of the SET_NODE or SET_SEG- MENT. SET_SEGMENT 1 NODE shared by two SET_SEGMENT SET_SEGMENT 2 7. Results including acoustic pressure and SPL are given in d3acs binary files, which can be accessed by LS-PrePost. Nodal pressure and SPL values for nodes specified by NID and NTYP are given in ASCII file Press_Pa and Press_dB, which can be accessed by LS-PrePost. Press_Pa gives magnitude of the pres- sure. Press_dB gives Sound Pressure Level in terms of dB. 8. If the boundary velocity condition is given by Steady State Dynamics (VAD = 0), the range and number of frequencies (FMIN, FMAX and NFREQ) should be compatible with the corresponding parameters in Card 1 of the key- word *FREQUENCY_DOMAIN_SSD 9. For acoustic eigenvalue analysis (OPTION = EIGENVALUE), Card 4 is optional and Card 5 is not used. *FREQUENCY_DOMAIN_ACOUSTIC_FRINGE_PLOT_{OPTION} Available options include: PART PART_SET NODE_SET SPHERE PLATE Purpose: Define field points for acoustic pressure computation by BEM acoustic solver, and save the results to D3ACS binary database. Card 1 for option PART, PART_SET or NODE_SET. Card 1 1 2 3 4 5 6 7 8 Variable PID/SID Type I Default none Card 1 for option SPHERE. Card 1 1 Variable CENTER Type Default I 1 2 R F 3 DENSITY I 4 X F 5 Y F 6 Z F 7 8 none none none none none Card 1 for option PLATE. Card 1 1 2 3 Variable NORM LEN_X LEN_Y Type Default I 1 F F 4 X F 5 Y F 6 Z F 7 8 NELM_X NELM_Y I I none none none none none 10 10 VARIABLE DESCRIPTION PID/SID Part ID or part set ID or node set ID. CENTER Flag for defining the center point for the sphere. EQ.1: mass center of the original structure. EQ.2: geometry center of the original structure. EQ.3: defined by (x, y, z). R Radius of the sphere. DENSITY Parameter to define how coarse or dense the created sphere mesh is. It is a number between 3 and 39, where “3” gives you 24 elements while “39” gives you 8664 elements. X Y Z x-coordinate of the center. y-coordinate of the center. z-coordinate of the center. NORM Norm direction of the plate. EQ.1: x-direction EQ.2: y-direction EQ.3: z-direction LEN_X Length of longer side of the plate. LEN_Y Length of shorter side of the plate. NELM_X Number of elements on longer side of the plate. NELM_Y Number of elements on shorter side of the plate. Remarks: 1. This command defines field points where the acoustic pressure will be computed by *FREQUENCY_DOMAIN_ACOUSTIC_BEM. The field points can be defined as existing structure components if option PART, PART_SET or NODE_SET is used. The field points can be created by LS-DYNA if option SPHERE or PLATE is used. 2. The acoustic pressure results at those field points are saved in D3ACS binary database and are accessible by LS-PrePost. With FCOMP tool in LS-PrePost, the fringe plot of the results (real part acoustic pressure, imaginary part acoustic pressure, magnitude of acoustic pressure and Sound Pressure Level) can be generated. 3. The field points defined by this keyword are separate from the field points defined in Card 2 of *FREQUENCY_DOMAIN_ACOUSTIC_BEM. The acoustic pressure results for the latter are only saved in ASCII database Press_Pa and Press_dB, etc. (in a tabular format that can be plotted in LS-PrePost by using the XYPlot tool). *FREQUENCY_DOMAIN_ACOUSTIC_INCIDENT_WAVE Purpose: Define incident sound wave for acoustic scattering problems. Wave Definition Cards. This card may be repeated to define multiple incident waves. Input stops when the next “*” Keyword is found. Card 1 1 2 Variable TYPE MAG Type Default I 1 F 6 7 8 3 XC F 4 YC F 5 ZC F none none none none VARIABLE DESCRIPTION TYPE Type of incident sound wave: EQ.1: plane wave. EQ.2: spherical wave. MAG Magnitude of the incident sound wave. GT.0: constant magnitude. LT.0: |MAG| is a curve ID, which defines the frequency dependent magnitude. See *DEFINE_CURVE. XC, YC, ZC Direction cosines for the place wave (TYPE = 1), or coordinates of the point source for the spherical wave (TYPE = 2). Remarks: 1. For plane wave, the incident wave is defined as 𝑝(𝑥, 𝑦, 𝑧) = 𝐴𝑒−𝑖𝑘(𝛼𝑥+𝛽𝑦+𝛾𝑧) where, 𝐴 is the magnitude of the incident wave and 𝛼, 𝛽 and 𝛾 are the direction cosines along the incident direction. 𝑖 = √−1 is the imaginary unit and 𝑘 = 𝜔/𝑐 is the wave number. 𝜔 is the round frequency and 𝑐 is the sound speed. 2. For spherical wave, the incident wave is defined as 𝑝(𝑟) = 𝐴 𝑒−𝑖𝑘𝑟 *FREQUENCY_DOMAIN_ACOUSTIC_INCIDENT_WAVE *FREQUENCY_DOMAIN where, 𝐴 is the magnitude of the incident wave and 𝑟 is the distance measured from the position of the point source. *FREQUENCY_DOMAIN_ACOUSTIC_SOUND_SPEED Purpose: Define frequency dependent complex sound speed to be used in frequency domain finite element method or boundary element method acoustic analysis. 2 3 4 5 6 7 8 Card 1 Variable 1 ID Type I Default none Card 2 1 2 3 4 5 6 7 8 Variable LCID1 LCID2 Type I I Default none none VARIABLE DESCRIPTION Complex sound speed ID. Curve ID for real part of frequency dependent complex sound speed. Curve ID for imaginary part of frequency dependent complex sound speed. ID LCID1 LCID2 Remarks: 1. The sound speed in an acoustic medium is usually defined as a constant real value. But it can also be defined as a complex value which is dependent on frequency, to introduce damping in the system. 2. To use the frequency dependent complex sound speed defined here, set the sound speed C = -ID in *FREQUENCY_DOMAIN_ACOUSTIC_FEM, or *FRE- QUENCY_DOMAIN_ACOUSTIC_BEM keywords. *FREQUENCY_DOMAIN_FRF Purpose: This keyword computes frequency response functions due to nodal excitations. NOTE: Natural frequencies and mode shapes are needed for computing the frequency response functions. Thus, *CONTROL_IMPLICIT_EIGENVALUE keyword must be included in input. See Remark 1. Card 1 Variable 1 N1 Type I Default none Card 2 1 2 3 4 5 6 7 8 N1TYP DOF1 VAD1 VID1 FNMAX MDMIN MDMAX I 0 2 I none 3 I 3 4 I 0 5 F 0.0 6 I 0 7 I 0 8 Variable DAMPF LCDAM LCTYP DMPMAS DMPSTF Type F Default 0.0 Card 3 Variable 1 N2 I 0 2 I 0 3 F F 0.0 0.0 4 5 6 7 8 N2TYP DOF2 VAD2 VID2 RELATV Type I Default none I 0 I none I 2 I 0 I Card 4 1 2 3 4 5 6 7 8 Variable FMIN FMAX NFREQ FSPACE LCFREQ RESTRT OUTPUT Type F F Default none none I 2 I 0 I none I 0 I 0 VARIABLE N1 DESCRIPTION Node / Node set/Segment set ID for excitation input. When VAD1, the excitation type, is set to 1, which is acceleration, this field is ignored. N1TYP Type of N1: EQ.0: node ID, EQ.1: node set ID, EQ.2: segment set ID. When VAD1, the excitation type, is set to 1, which is acceleration, this field is ignored. DOF1 Applicable degrees-of-freedom for excitation input (ignored if VAD1 = 4): EQ.0: translational movement in direction given by vector VID1, EQ.1: x-translational degree-of-freedom, or x-rotational degree-of-freedom (for torque excitation, VAD1 = 8) EQ.2: y-translational degree-of-freedom, or y-rotational degree-of-freedom (for torque excitation, VAD1 = 8), EQ.3: z-translational degree-of-freedom, or z-rotational degree-of-freedom (for torque excitation, VAD1 = 8). VARIABLE DESCRIPTION VAD1 Excitation input type: EQ.0: base velocity, EQ.1: base acceleration, EQ.2: base displacement, EQ.3: nodal force, EQ.4: pressure, EQ.5: enforced velocity by large mass method, EQ.6: enforced acceleration by large mass method, EQ.7: enforced displacement by large mass method. EQ.8: torque, EQ.9: base angular velocity, EQ.10: EQ.11: base angular acceleration, base angular displacement VID1 FNMAX MDMIN MDMAX Vector ID for DOF1 = 0 for excitation input, see *DEFINE_VEC- TOR. Optional maximum natural computation. See Remark 3. frequency employed in FRF The first mode employed in FRF computation (optional). See Remarks 3 and 4. The last mode employed in FRF computation (optional). It should be set as a positive integer in a restart run (RESTRT = 1 or 3) based on the number of eigenmodes available in the existing d3eigv database. See Remarks 3 and 4. DAMPF Modal damping coefficient, 𝜁 . See Remark 5. LCDAM Load Curve ID defining mode dependent modal damping coefficient, 𝜁 . See Remark 5. LCTYP Type of load curve defining modal damping coefficient: EQ.0: Abscissa value defines frequency, EQ.1: Abscissa value defines mode number. See Remark 5. VARIABLE DMPMAS DESCRIPTION Mass proportional damping constant, 𝛼, in Rayleigh damping. See Remark 5. DMPSTF Stiffness proportional damping constant, 𝛽, in Rayleigh damping. See Remark 5. N2 Node / Node set/Segment set ID for response output. N2TYP Type of N2: EQ.0: node ID, EQ.1: node set ID, EQ.2: segment set ID. DOF2 Applicable degrees-of-freedom for response output: EQ.0: direction given by vector VID2, EQ.1: 𝑥-translational degree-of-freedom, EQ.2: 𝑦-translational degree-of-freedom, EQ.3: 𝑧-translational degree-of-freedom, EQ.4: 𝑥-rotational degree-of-freedom, EQ.5: 𝑦-rotational degree-of-freedom, EQ.6: 𝑧-rotational degree-of-freedom, EQ.7: 𝑥, 𝑦 and 𝑧-translational degrees-of-freedom, EQ.8: 𝑥, 𝑦 and 𝑧-rotational degrees-of-freedom. VAD2 Response output type: EQ.0: velocity, EQ.1: acceleration, EQ.2: displacement, EQ.3: nodal force . VID2 Vector ID for DOF2 = 0 for response direction, see *DEFINE_- VECTOR. RELATV FLAG for displacement, velocity and acceleration results: EQ.0: absolute values are requested, EQ.1: relative values are requested (for VAD1 = 0, 1, 2 only). VARIABLE DESCRIPTION FMIN FMAX Minimum frequency for FRF output (cycles/time). See Remark 6. Maximum frequency for FRF output (cycles/time). See Remark 6. NFREQ Number of frequencies for FRF output. See Remark 6. FSPACE Frequency spacing option for FRF output: EQ.0: linear, EQ.1: logarithmic, EQ.2: biased. See Remark 6. LCFREQ Load Curve ID defining the frequencies for FRF output. See Remark 6. RESTRT Restart option: EQ.0: initial run, EQ.1: restart with d3eigv family files, EQ.2: restart with dumpfrf, EQ.3: restart with d3eigv family files and dumpfrf. See Remark 7. OUTPUT Output option: EQ.0: write amplitude and phase angle pairs, EQ.1: write real and imaginary pairs. Remarks: 1. Frequency Response Functions. The FRF (frequency response functions) can be given as Displacement/Force (called Admittance, Compliance, or Re- ceptance), Velocity/Force (called Mobility), Acceleration/Force (called Acceler- ance, Inertance), etc. 2. Enforced Motion. The excitation input can be given as enforced motion (VAD1 = 5, 6, 7). Large mass method is used for this type of excitation input. The user need to attach a large mass to the nodes where the enforced motion is applied by using the keyword *ELEMENT_MASS_{OPTION}, and report the keyword large (MPN) node mass per the in *CONTROL_FREQUENCY_DOMAIN. *CONTROL_FREQUENCY_DOMAIN. For more details, please refer to 3. Maximum Frequency. FNMAX decides how many natural vibration modes are adopted in FRF computation. LS-DYNA uses only modes with lower or equal frequency than FNMAX in FRF computation. If FNMAX is not given, the number of modes in FRF computation is same as the number of modes, NEIG, from the *CONTROL_IMPLICIT_EIGENVALUE keyword card, unless MDMIN and MDMAX are prescribed . 4. Maximum/Minimum Mode. MDMIN and MDMAX decide which mode(s) are adopted in FRF computation. This option is useful for calculating the contribu- tion from a single mode (MDMIN = MDMAX) or several modes (MDMIN < MDMAX). If only MDMIN is given, LS-DYNA uses the single mode (MDMIN) to compute FRF. In a restart run based on existing eigenmode database d3eigv (RESTRT = 1 or 3), MDMAX should be a positive integer which is equal to or less than the number of eigenmodes available in d3eigv. 5. Damping. Damping can be prescribed in several ways: a) To use a constant modal damping coefficient ζ for all the modes, define DAMPF only. LCDMP, LCTYP, DMPMAS and DMPSTF are ignored. b) To use mode dependent modal damping, define a load curve (*DEFINE_- CURVE) and specify that if the abscissa value defines the frequency or mode number by LCTYP. DMPMAS and DMPSTF are ignored. c) To use Rayleigh damping, define DMPMAS (𝛼) and DMPSTF (𝛽) and keep DAMPF as 0.0, and keep LCDMP, LCTYP as 0. The damping matrix in Rayleigh damping is defined as 𝐂 = 𝛼𝐌 + 𝛽𝐊, where, 𝐂, 𝐌 and 𝐊 are the damping, mass and stiffness matrices respectively. fmin fmin fmin Linear Spacing Logarithmic Spacing fmax fmax mode n mode n+1 mode n+2 Biased Spacing fmax Figure 20-2. Spacing options of the frequency points. 6. Frequency Points. There are two methods to define the frequencies. a) The first method is to define FMIN, FMAX, NFREQ and FSPACE. FMIN and FMAX specify the frequency range of interest and NFREQ specifies the number of frequencies at which results are required. FSPACE speci- fies the type of frequency spacing (linear, logarithmic or biased) to be used. These frequency points for which results are required can be spaced equally along the frequency axis (on a linear or logarithmic scale). Or they can be biased toward the eigenfrequencies (the frequency points are placed closer together at eigenfrequencies in the frequency range) so that the detailed definition of the response close to resonance frequencies can be obtained. See Figure 20-2. b) The second method is to use a load curve (LCFREQ) to define the frequen- cies of interest. 7. RESTRT Field. To save time in subsequent runs, the modal analysis stored in the d3eigv file during the first run can be reused by setting RESTRT=1. RESTRT = 2 or 3 is used when user wants to add extra vibration modes to FRF computation. After initial FRF computation, user may find that the number of vibration modes is not enough. For example, in the initial computation, user may use only vibration modes up to 500 Hz. Later it is found that vibration modes at higher frequencies are needed. Then it would be more efficient to just compute the extra modes (frequencies above 500 Hz), and add the contribution from these extra modes to the previous FRF results. In this case, user may use the option RESTRT = 2 or 3. For RESTRT = 2, LS- DYNA runs a new modal analysis, reads in the previous FRF results (stored in the binary dump file dumpfrf), and add the contribution from the new modes. For RESTRT = 3, LS-DYNA reads in d3eigv family files generated elsewhere and reads in also dumpfrf, and add the contribution from the new modes. 8. Nodal Force Response Output. For nodal force response (VAD2=3), the same nodes or node set need to be defined in *DATABASE_NODAL_FORCE_- GROUP. In addition the MSTRES field for the *CONTROL_IMPLICIT_EIGEN- VALUE keyword must be set to 1. *FREQUENCY_DOMAIN_MODE_{OPTION1}_{OPTION2} Available options for OPTION1 include: LIST GENERATE SET For OPTION2 the available option is: EXCLUDE Purpose: Define vibration modes to be used in modal superposition, modal acceleration or modal combination procedures for mode-based frequency domain analysis (such as frequency response functions, steady state dynamics, random vibration analysis and response spectrum analysis). When the option2 EXCLUDE is used, the modes defined in this keyword are excluded from participating in the modal superposition, modal acceleration or modal combination procedures. Mode ID Cards. For LIST keyword option list the mode IDs. Include as many cards as necessary. This input ends at the next keyword (“*”) card. Card 1 1 2 3 4 5 6 7 8 Variable MID1 MID2 MID3 MID4 MID5 MID6 MID7 MID8 Type I I I I I I I I Mode Block Cards. For GENERATE keyword option specify ranges of modes. Include as many cards as necessary. This input ends at the next keyword (“*”) card. Card 1 1 2 3 4 5 6 7 8 Variable M1BEG M1END M2BEG M2END M3BEG M3END M4BEG M4END Type I I I I I I I Mode Set Card. For SET keyword option specify a mode set. Include only one card. Card 1 1 2 3 4 5 6 7 8 Variable SID Type I VARIABLE DESCRIPTION MIDn Mode ID n. MnBEG First mode ID in block n. MnEND Last mode ID in block n. All mode ID’s between and including MnBEG and MnEND are added to the list. SID Mode set identification . Remarks: 1. User may use this keyword if some of the vibration modes have less contribu- tion to the total structural response and can be removed from the modal super- position, modal acceleration or modal combination procedures in the mode- based frequency domain analysis. 2. The mode list defined by this keyword overrides the modes specified by MD- MIN, MDMAX (or FNMIX, FNMAX) in the keywords *FREQUENCY_DO- MAIN_FRF, *FREQUENCY_DOMAIN_SSD, etc. *FREQUENCY_DOMAIN_PATH_{OPTION} Available options include: <BLANK> PARTITION Purpose: Specify the path and file name of binary databases (e.g. d3eigv) containing mode information for restarting frequency domain analyses such as FRF, SSD, Random vibration, and Response spectrum analysis. The PARTITION option supports assigning different binary databases to different frequency ranges. Specifically, each frequency range can be associated with different eigenmodes and modal shape vectors provided by the binary database. This option provides a model for materials that have frequency-dependent properties. Partition Cards. Card 1 for the PARTITION keyword option. Include one card for each frequency range. This input ends at the next keyword (“*”) card. Card 1 1 2 3 4 5 6 7 8 Variable FBEG FEND FILENAME Type F F Default none none C none Filename Card. Card 1 format used with the keyword option left blank. Card 1 1 2 3 4 5 6 7 8 Variable Type Default FILENAME C none VARIABLE DESCRIPTION FBEG FEND Beginning frequency for using this database Ending frequency for using this database FILENAME Path and name of information. the database which contains modal Remarks: 1. If the binary database files are in the runtime directory, this card is not needed for the case without partitioning. 2. When the option PARTITION is active, the binary database designated by FILENAME is used for the frequency range starting from (and including) FBEG and ending at (not including) FEND. *FREQUENCY_DOMAIN_RANDOM_VIBRATION Available options include: <BLANK> FATIGUE Purpose: Set random vibration control options. When FATIGUE option is used, compute fatigue life of structures or parts under random vibration. Card 1 1 2 3 4 5 6 7 8 Variable MDMIN MDMAX FNMIN FNMAX RESTRT RESTRM Type Default I 1 I F F 0.0 Card 2 1 2 3 4 I 0 5 6 I 0 7 8 Variable DAMPF LCDAM LCTYP DMPMAS DMPSTF DMPTYP Type F Default 0.0 Card 3 1 I 0 2 I 0 3 F F 0.0 0.0 4 5 I 0 6 7 8 Variable VAFLAG METHOD UNIT UMLT VAPSD VARMS NAPSD NCPSD Type I Default none I 0 I F I I I 1 I Card 4 1 2 3 4 5 6 7 8 Variable LDTYP IPANELU IPANELV TEMPER LDFLAG Type I I I F Default 0.0 I 0 Auto PSD Cards. Include NAPSD cards of this format, one per excitation. Card 5a 1 2 3 4 5 6 7 8 Variable SID STYPE DOF LDPSD LDVEL LDFLW LDSPN CID Type I I I I Default I 0 I 0 I 0 I 0 Cross PSD Cards. Include NCPSD cards of this format, one per excitation. Card 5b 1 2 3 4 5 6 7 8 Variable LOAD_I LOAD_J LCTYP2 LDPSD1 LDPSD2 Type I I Default I I I Fatigue Card. Additional card for FATIGUE keyword option. Card 6 1 2 3 4 5 6 7 8 Variable MFTG NFTG SNTYPE TEXPOS STRSF INFTG Type Default I 0 I 1 I 0 F F 0.0 1.0 I 0 S-N Curve Cards. NFTG additional cards for FATIGUE keyword option. Each Card 7 defines one zone for fatigue analysis and the corresponding S-N fatigue curve for that zone. Card 7 1 2 3 4 Variable PID LCID PTYPE LTYPE Type I I Default I 0 I 0 5 A F 6 B F 7 8 STHRES SNLIMT F 0. I 0 Initial Damage Card. INFTG additional cards for FATIGUE keyword option when INFTG > 0. Card 8 1 2 3 4 5 6 7 8 Variable Type Default FILENAME C d3ftg VARIABLE DESCRIPTION MDMIN The first mode in modal superposition method (optional). MDMAX The last mode in modal superposition method (optional). VARIABLE FNMIN DESCRIPTION The minimum natural frequency in modal superposition Method (optional). FNMAX The maximum natural frequency in modal superposition method (optional). RESTRT Restart option. EQ.0: A new modal analysis is performed, EQ.1: Restart with d3eigv. RESTRM Restart option when different types of loads are present. EQ.0: don’t read the dump file for PSD and RMS, EQ.1: read in PSD and RMS values from the dump file and add them to the values computed in the current load case. DAMPF LCDAM Modal damping coefficient, ζ. Load Curve ID defining mode dependent modal damping coefficient ζ. LCTYP Type of load curve defining modal damping coefficient EQ.0: Abscissa value defines frequency, EQ.1: Abscissa value defines mode number. DMPMAS Mass proportional damping constant 𝛼, in Rayleigh damping. DMPSTF Stiffness proportional damping constant 𝛽, in Rayleigh damping. DMPTYP Type of damping EQ.0: modal damping. EQ.1: broadband damping. VARIABLE DESCRIPTION VAFLAG Loading type: EQ.0: No random vibration analysis. EQ.1: Base acceleration. EQ.2: Random pressure. EQ.3: Plane wave. EQ.4: Shock wave. EQ.5: Progressive wave. EQ.6: Reverberant wave. EQ.7: Turbulent boundary layer wave. EQ.8: Nodal force. METHOD Method for modal response analysis. EQ.0: method set automatically by LS-DYNA (recommended) EQ.1: modal superposition method EQ.2: modal acceleration method EQ.3: modal truncation augmentation method UNIT Flag for acceleration unit conversion: EQ.0: use [length unit]/[time unit]2 as unit of acceleration. EQ.1: use g as unit for acceleration, and SI units (Newton, kg, meter, second, etc.) elsewhere. EQ.2: use g as unit for acceleration, and Engineering units (lbf, lbf × second2/inch, inch, second, etc.) elsewhere. EQ.3: use g as unit for acceleration, and units (kN, kg, mm, ms, GPa, etc.) elsewhere. EQ.-1: use g as unit for acceleration and provide the multiplier for converting g to [length unit]/[time unit]2. UMLT Multiplier for converting g to [length unit]/[time unit]2 (used only for UNIT = -1). VARIABLE DESCRIPTION VAPSD Flag for PSD output: EQ.0: Absolute PSD output is requested. EQ.1: Relative PSD output is requested (used only for VAFLAG = 1) VARMS Flag for RMS output: EQ.0: Absolute RMS output is requested. EQ.1: Relative RMS output is requested (used only for VAFLAG = 1) NAPSD NCPSD Number of auto PSD load definition. Card 5a is repeated “NAPSD” times, one for each auto PSD load definition. The default value is 1. Number of cross PSD load definition. Card 5b is repeated “NCPSD” times, one for each cross PSD load definition. The default value is 0. LDTYP Excitation load (LDPSD in card 5) type: EQ.0: PSD. EQ.1: SPL (for plane wave only). EQ.2: time history load. IPANELU Number of strips in U direction (used only for VAFLAG = 5, 6, 7) IPANELV Number of strips in V direction (used only for VAFLAG = 5, 6, 7) TEMPER Temperature LDFLAG Type of loading curves. EQ.0: Log-Log interpolation (default) EQ.1: Semi-Log interpolation EQ.2: Linear-Linear interpolation VARIABLE SID DESCRIPTION GE.0: Set ID for the panel exposed to acoustic environment, or the nodes subjected to nodal force excitation, or nodal acceleration excitation. For VAFLAG = 1, base accelera- tion, leave this as blank LT.0: used to define the cross-PSD. |SID| is the ID of the load cases. STYPE Flag specifying meaning of SID. EQ.0: Node EQ.1: Node Set EQ.2: Segment Set EQ.3: Part EQ.4: Part Set LT.0: used to define the cross-psd. |STYPE| is the ID of the load cases. DOF Applicable degrees-of-freedom for nodal force excitation or base acceleration (DOF = 1, 2, and 3), or wave direction: EQ.0: translational movement in direction given by vector VID. EQ.±1: x-translational degree-of-freedom (positive or negative) EQ.±2: y-translational degree-of-freedom (positive or negative) EQ.±3: z-translational degree-of-freedom (positive or negative) LDPSD Load curve for PSD, SPL, or time history excitation. LDVEL Load curve for phase velocity. LDFLW Load curve for exponential decay for TBL in flow-wise direction LDSPN Load curve for exponential decay for TBL in span-wise direction CID/VID Coordinate system ID for defining wave direction, see *DEFINE_- COORDINATE_SYSTEM; or Vector ID for defining load direction for nodal force, or base excitation, see *DEFINE_VECTOR. LOAD_I ID of load i for cross PSD. LOAD_J ID of load j for cross PSD. VARIABLE LCTYP2 DESCRIPTION Type of load curves (LDPSD1 and LDPSD2) for defining cross PSD: EQ.0: LDPSD1 defines real part and LDPSD2 defines imaginary part EQ.1: LDPSD1 defines magnitude and LDPSD2 defines phase angle LDPSD1 Load curve for real part or magnitude of cross PSD LDPSD2 Load curve for imaginary part or phase angle of cross PSD MFTG Method for random fatigue analysis (for option_FATIGUE). EQ.0: no fatigue analysis, EQ.1: Steinberg’s three-band method, EQ.2: Dirlik method, EQ.3: Narrow band method, EQ.4: Wirsching method, EQ.5: Chaudhury and Dover method, EQ.6: Tunna method, EQ.7: Hancock method. NFTG Field specifying the number of S - N curves to be defined. GE.0: Number of S - N curves defined by card 6. Card 6 is repeated “NFTG” number of times, one for each S - N fatigue curve definition. The default value is 1. EQ.-999: S - N curves are defined through *MAT_ADD_FA- TIGUE. If the option FATIGUE is not used, ignore this parameter. SNTYPE Stress type of S - N curve in fatigue analysis. EQ.0: von-mises stress EQ.1: maximum principal stress (not implemented) EQ.2: maximum shear stress (not implemented) EQ.-n: The nth stress component. TEXPOS Exposure time (used if option FATIGUE is used) VARIABLE STRSF DESCRIPTION Stress scale factor to accommodate different ordinates in S - N curve. EQ.1: used if the ordinate in S - N curve is stress range (default) EQ.2: used if the ordinate in S - N curve is stress amplitude INFTG Flag for including initial damage ratio. EQ.0: no initial damage ratio, GT.0: read existing d3ftg files to get initial damage ratio. When INFTG > 1, it means that the initial damage ratio comes from multiple loading cases (correspondingly, multiple binary databases, defined by Card 7). The value of INFTG should be ≤ 10. PID Part ID, or Part Set ID, or Element (solid, shell, beam, thick shell) Set ID. LCID S - N fatigue curve ID for the current Part or Part Set. GT.0: S - N fatigue curve ID EQ.-1: S - N fatigue curve uses equation 𝑁𝑆𝑏 = 𝑎 EQ.-2: S - N fatigue curve uses equation log(𝑆) = 𝑎 − 𝑏 log(𝑁) EQ.-3: S - N fatigue curve uses equation 𝑆 = 𝑎 𝑁𝑏 PTYPE Type of PID. EQ.0: Part (default) EQ.1: Part Set EQ.2: SET_SOLID EQ.3: SET_BEAM EQ.4: SET_SHELL EQ.5: SET_TSHELL LTYPE Type of LCID. EQ.0: Semi-log interpolation (default) EQ.1: Log-Log interpolation EQ.2: Linear-Linear interpolation VARIABLE DESCRIPTION A B Material parameter 𝑎 in S - N fatigue equation. Material parameter 𝑏 in S - N fatigue equation. STHRES Fatigue threshold (applicable only if LCID < 0). SNLIMT If LCID > 0 Flag setting algorithm used when stress is lower than the lowest stress on S - N curve (if LCID > 0), or lower than STHRES (if LCID < 0). EQ.0: use the life at the last point on S - N curve EQ.1: extrapolation from the last two points on S - N curve (only applicable if LCID > 0) EQ.2: infinity. If LCID < 0 Flag setting algorithm used when stress is lower STHRES EQ.0: use the life at STHRES EQ.1: Ingnored. only applicable for LCID > 0 EQ.2: infinity. FILENAME Path and name of existing binary database information. for fatigue Remarks: 1. Historical Background. This command evaluates the structural random vibration response due to aero acoustic loads, base excitation, or nodal force. This capability originated in Boeing’s in-house code N-FEARA, which is a NI- KE3D-based Finite Element tool for performing structural analysis with vibro- acoustic loads. The main developer of N-FEARA is Mostafa Rassaian from the Boeing Company. 2. Fatigue. To run this option, it is required that MSTRES = 1 in the keyword *CONTROL_IMPLICIT_EIGENVALUE. This is because the fatigue analysis is depends on stresses. 3. IPANEL. The number of strips the in U and V direction are used to group the elements and thereby reduce the number integration domains reducing compu- tational expense. This option is only available for VAFLAG = 5, 6, and 7. 4. Restarting. Restart option RESTRT = 1 is used when mode analysis has been done previously. In this case, LS-DYNA skips modal analysis and reads in the d3eigv files from the prior execution. For RESTMD = 1, always use MDMIN = 1 and set MDMAX to the number of modes in the previous run (this can be found in the ASCII file eigout, or it can be extracted from the d3eigv files using LS- PrePost). 5. Accumulated Fatigue. The fatigue damage ratio can be accumulated over multiple load cases by setting INFTG = 1. This is useful when a structure is subjected to multiple independent random vibrations. LS-DYNA calculates the total damage ratio by adding the damage ratio from the current calculation to the damage ratio of the previous calculation which are stored in the previous calculation’s fatigue database (d3ftg by default). The previous d3ftg file will be overwritten by the new one, if it is in the same directory. 6. Automatic Method Selection. If METHOD = 0, LS-DYNA uses modal superposition method for cases (VAFLAG) 4, 5, 6, 7; For cases 1, 2, 3 and 8, LS- DYNA uses modal superposition method when preload condition is present and uses modal acceleration method when preload condition is not present. 7. Units. In a set of consistent units, the unit for acceleration is defined as 1 (acceleration unit) = 1(length unit) [1(time unit)]2 Some users in industry prefer to use g (acceleration due to gravity) as the unit for acceleration. For example, 1g = 9.81 s2 = 386.089 inch s2 If the input and output use g as the unit for acceleration, select UNIT = 1, 2, or 3. If UNIT = 3, a multiplier (UMLT) for converting g to [length unit]/[time unit]2 is needed and it is defined by 1g = UMLT × [length unit] [time unit]2 For more information about the consistent units, see GS.21 (GETTING START- ED). 8. Restrictions on Load Curves. The load curves LDPSD, LDVEL, LDFLW, and LDSPN must all be defined using the same number of points. The number of points in the load curve LDDAMP can be different from those for LDPSD, LDVEL, LDFLW, and LDSPN. 9. Wave direction. Wave direction is determined DOF and CID/VID. CID/VID represents a local U-V-W coordinate system for defining acoustic wave direc- tion, only partially correlated waves (VAFLAG=5, 6, 7) need this local coordi- nate system. For nodal force, base excitation, plane wave or random pressure, CID represents a vector ID defining the load direction (DOF = ±4). 10. Stress / Strain computation. To get stress results (PSD and RMS) from random vibration analysis, MSTRES field of the *CONTROL_IMPLICIT_- EIGENVALUE keyword should be set to 1. To get strain results (PSD and RMS) the STRFLG field of *DATABASE_EXTENT_BINARY should be set to 1. To get stress component results for beam elements (which are not based on resultant formulation), the BEAMIP field of *DATABASE_EXTENT_BINARY should be set greater than 0. 11. Binary plot databases. PSD and RMS results are given for all nodes and elements. PSD results are written in binary to a file named d3psd. Similarly, RMS results are written in binary to a file named d3rms. See the keyword *DATABASE_FREQUENCY_BINARY_{OPTION} for more details. 12. ASCII Output for Displacement. Displacement, velocity, and acceleration PSD results are output into ASCII file nodout_psd. The set nodes for which data is written to nodout_psd is specified with the *DATABASE_HISTORY_- NODE keyword. 13. ASCII Output for Stress. Stress PSD results are output into ASCII file elout_ psd. The set of solid, beam, shell, and thick shell elements to be written to the elout_psd file are specified with the following keywords: *DATABASE_HISTO- RY_SOLID, *DATABASE_HISTORY_BEAM, *DATABASE_HISTORY_SHELL, *DATABASE_HISTORY_TSHELL. 14. Cross PSD. The cross PSD can be defined as complex variables to consider phase difference. In that case, two curves are needed to define the cross PSD (LCPSD1 and LCPSD2). Two load IDs are needed to define the cross PSD (LOAD_I and LOAD_J). They are simply the ordering numbers by which the auto PSDs are defined. For example, the first Card 5a defines load 1 and the second Card 5a defines the load 2. No cross PSD is required if two loads are uncorrelated. Cross PSD for any pair of two correlated loads is defined only once – from lower load ID to higher load ID (e.g. 1->2, 1->3, 2->3, …). The cross PSD from higher load ID to lower load ID (e.g. 2->1, 3->1, 3->2, …) is added by LS-DYNA automatically by using the relationship ̅̅̅̅̅̅̅̅̅ 𝐺𝑗𝑖 = 𝐺𝚤𝚥 where 𝐺𝑖𝑗 is the cross PSD from load i to load j, and ̅̅̅̅̅̅̅ represents the complex conjugate. 15. Cross Correlation. Cross correlation can be defined only for same type of excitations (e.g. nodal force, random pressure). Correlation between different types of excitations is not allowed 16. Output for Fatigue Data. When the FATIGUE option is used, a binary plot file, d3ftg, is written. 5 results are included in d3ftg: Result 1. Cumulative damage ratio Result 2. Expected fatigue life Result 3. Zero-crossing frequency Result 4. Peak-crossing frequency Result 5. Irregularity factor These results are given as element variables. Irregularity factor is a real number from 0 to 1. A sine wave has irregularity factor as 1, while white noise has irregularity factor as 0. The lower the irregularity factor, the closer the process is to the broad band case. 17. Stress Threshold for Fatigue. In some materials, the S−N curve flattens out eventually, so that below a certain threshold stress STHRES failure does not occur no matter how long the loads are cycled. SNLIMT can be set to 2 in this case; For other materials, such as aluminum, no threshold stress exists and SNLIMT should be set to 0 or 1 for added level of safety. 18. Restriction on Fatigue Cards. When the FATIGUE option is used, all fatigue cards (Card 6) must be of the same PTYPE (PART or SET of ELEMENTS). 19. Format for S - N Curves. S - N curves can be defined by *DEFINE_CURVE, or for LCID<0 by when LCID = -1 or for LCID = -2 𝑁𝑆𝑏 = 𝑎 or for LCID = -3 log(𝑆) = 𝑎 − 𝑏 log(𝑁) 𝑆 = 𝑎 𝑁𝑏 where N is the number of cycles for fatigue failure and S is the stress amplitude. Please note that the two equations can be converted to each other, with some minor manipulation on the constants a and b. References: Mostafa Rassaian, Jung-Chuan Lee, N-FEARA – NIKE3D-based FE tool for structural analysis of vibro-acoustic loads, Boeing report, 9350N-GKY-02-036, December 5, 2003. *FREQUENCY_DOMAIN_RESPONSE_SPECTRUM Purpose: perform response spectrum computation to obtain the peak response of a structure. Card 1 1 2 3 4 5 6 7 8 Variable MDMIN MDMAX FNMIN FNMAX RESTRT MCOMB Type Default I 1 I F F 0.0 Card 2 1 2 3 4 I 0 5 I 0 6 7 8 Variable DAMPF LCDAMP LDTYP DMPMAS DMPSTF Type F I Default none none I 0 F F 0.0 0.0 Card 3 can be repeated if 2 or more input spectra exist (multiple-point response spectrum) Card 3 1 2 3 Variable LCTYP DOF LC/TBID Type I I I Default 4 SF F 1.0 5 6 7 8 VID LNID LNTYP INFLAG I I I I 0 VARIABLE DESCRIPTION MDMIN MDMAX The first mode in modal superposition method (optional). The last mode in modal superposition method (optional). FNMIN FNMAX The minimum natural frequency in modal superposition method (optional). The maximum natural frequency in modal superposition method (optional). RESTRT Restart option EQ.0: A new run including modal analysis, EQ.1: Restart with d3eigv family files created elsewhere. MCOMB Method for combination of modes: EQ.0: SRSS method, EQ.1: NRC Grouping method, EQ.2: Complete Quadratic Combination method (CQC), EQ.3: Double Sum method based on Rosenblueth-Elorduy coefficient, EQ.4: NRL-SUM method, EQ.5: Double Sum method based on Gupta-Cordero coefficient, EQ.6: Double Sum method based on modified Gupta-Cordero coefficient, EQ.7: Rosenblueth method. DAMPF Modal damping ratio, ζ. LCDAMP Load Curve ID for defining frequency dependent modal damping ratio ζ. LDTYP Type of load curve for LCDAMP EQ.0: Abscissa value defines frequency, EQ.1: Abscissa value defines mode number. DMPMAS Mass proportional damping constant α, in Rayleigh damping. DMPSTF Stiffness proportional damping constant β, in Rayleigh damping. LCTYP Load curve type for defining the input spectrum. EQ.0: base velocity, EQ.1: base acceleration, EQ.2: base displacement, EQ.3: nodal force, EQ.4: pressure, EQ.10: base velocity time history, EQ.11: base acceleration time history, EQ.12: base displacement time history. DOF Applicable degrees-of-freedom for excitation input: EQ.1: x-translational degree-of-freedom, EQ.2: y-translational degree-of-freedom, EQ.3: z-translational degree-of-freedom, EQ.4: translational movement in direction given by vector VID. Load curve or table ID, see *DEFINE_TABLE, defining the response spectrum for frequencies. If the table definition is used a family of curves are defined for discrete critical damping ratios. Scale factor for the input load spectrum. Vector ID for DOF values of 4. Node ID, or node set ID, or segment set ID where the excitation is applied. If the input load is given as base excitation spectrum, LNID = 0 LC/TBID SF VID LNID LNTYP Set type for LNID: EQ.1: Node, see *NODE, EQ.2: Node set, see *SET_NODE, EQ.3: Segment set, see *SET_SEGMENT, EQ.4: Part, see *PART, EQ.5: Part set, see *SET_PART. INFLAG Frequency interpolation option EQ.0: Logarithmic interpolation, EQ.1: Semi-logarithmic interpolation. EQ.2: Linear interpolation. Remarks: 1. This command uses modal superposition method to evaluate the maximum response of a structure subjected to input response spectrum load, such as the acceleration spectrum load in earthquake engineering. 2. Modal analysis has to be performed preceding the response spectrum analysis. Thus the keywords *CONTROL_IMPLICIT_GENERAL and *CONTROL_IM- PLICIT_EIGENVALUE are expected in the input file. 3. MDMIN, MDMAX, FNMIN and FNMAX should be set appropriately to cover all the natural modes inside the input spectrum. 4. To include stress results, modal stress computation has to be requested in *CONTROL_IMPLICIT_EIGENVALUE (set MSTRES = 1). 5. For base excitation cases, user can choose relative values or absolute values for displacement, velocity and acceleration results output. 6. RESTRT = 1 enables a fast restart run based on d3eigv family files generated in last run or elsewhere. LS-DYNA reads d3eigv family files to get the natural vibration frequencies and mode shapes. If the d3eigv family files are located in a directory other than the working directory, the directory must be specified in *FREQUENCY_DOMAIN_PATH. 7. For Double Sum method (MCOMB = 3), earthquake duration time is given by ENDTIM in the keyword *CONTROL_TERMINATION. 8. Three interpolation options are available for frequency interpolation when reading response spectrum values a) When INFLAG = 0 (default), logarithmic interpolation is used, e.g. log𝑦 − log𝑦1 log𝑥 − log𝑥1 = log𝑦2 − log𝑦1 log𝑥2 − log𝑥1 b) When INFLAG = 1, semi-logarithmic interpolation is used, e.g. log𝑦 − log𝑦1 𝑥 − 𝑥1 = log𝑦2 − log𝑦1 𝑥2 − 𝑥1 c) When INFLAG = 2, linear interpolation is used, e.g. 𝑦 − 𝑦1 𝑥 − 𝑥1 𝑦2 − 𝑦1 𝑥2 − 𝑥1 = 9. Linear interpolation is used for interpolation with respect to damping ratios. *FREQUENCY_DOMAIN_SSD_{OPTION} Available options include: FATIGUE ERP Purpose: Compute steady state dynamic response due to given spectrum of harmonic excitations. When the FATIGUE option is applied LS-DYNA also calculates the cumulative fatigue damage ratio. When the ERP option is applied LS-DYNA also calculates the Equivalent Radiated Power (ERP) due to vibration. Card 1 1 2 3 4 5 6 7 8 Variable MDMIN MDMAX FNMIN FNMAX RESTMD RESTDP LCFLAG RELATV Type Default I 1 I F F 0.0 Card 2 1 2 3 4 I 0 5 I 0 6 I 0 7 I 0 8 Variable DAMPF LCDAM LCTYP DMPMAS DMPSTF DMPFLG Type F Default 0.0 Card 3 1 I 0 2 I 0 3 F F 0.0 0.0 4 5 I 0 6 7 8 Variable Type Default MEMORY NERP STRTYP NOUT NOTYP NOVA I 0 I 0 I 0 I 0 I 0 I ERP Card. This card is read only when the ERP option is active. Card 4a Variable 1 RO Type F 2 C F 3 4 5 6 7 8 ERPRLF ERPREF F F Default none none 1.0 0.0 ERP Part Cards. This card is read NERP times. Since NERP defaults to zero this card is, by default not read, and, furthermore, it is not read unless the ERP option is active. Card 5 1 2 3 4 5 6 7 8 Variable PID PTYP Type I Default none I 0 Excitation Loads. Repeat Card 4 if multiple excitation loads are present. Card 4 1 2 3 4 5 6 7 Variable NID NTYP DOF VAD LC1 LC2 LC3 Type I Default none I 0 I I I I none none none none I 0 8 VID I 0 VARIABLE DESCRIPTION MDMIN The first mode in modal superposition method (optional). MDMAX The last mode in modal superposition method (optional). FNMIN The minimum natural frequency in modal superposition method (optional). VARIABLE FNMAX DESCRIPTION The maximum natural frequency in modal superposition method (optional). RESTMD Restart option: EQ.0: A new modal analysis is performed, EQ.1: Restart with d3eigv. RESTDP Restart option: EQ.0: A new run without dumpssd, EQ.1: Restart with dumpssd. LCFLAG Load Curve definition flag. EQ.0: load curves are given as amplitude / phase angle, EQ.1: load curves are given as real / imaginary components. RELATV Flag for displacement, velocity and acceleration results: EQ.0: absolute values are requested, EQ.1: relative values are requested (for VAD = 2, 3 and 4 only). DAMPF LCDAM Modal damping coefficient, ζ. Load Curve ID defining mode dependent modal damping coefficient ζ. LCTYP Type of load curve defining modal damping coefficient. EQ.0: Abscissa value defines frequency, EQ.1: Abscissa value defines mode number. DMPMAS Mass proportional damping constant 𝛼, in Rayleigh damping. DMPSTF Stiffness proportional damping constant 𝛽, in Rayleigh damping DMPFLG Damping flag: EQ.0: use modal damping coefficient 𝜁 , defined by DAMPF, or LCDAM, or Rayleigh damping defined by DMPMAS and DMPSTF in this card. EQ.1: use damping defined by *DAMPING_PART_MASS and *DAMPING_PART_STIFFNESS. VARIABLE DESCRIPTION MEMORY Memory flag: EQ.0: modal superposition will be performed in-core. This option runs faster. EQ.1: modal superposition will be performed out-of-core. This is needed for some large scale problems that cannot fit in main memory. This method incurs a performance penal- ty associated with disk speed. NERP Number of ERP panels. STRTYP Stress used in fatigue analysis: EQ.0: Von Mises stress, EQ.1: Maximum principal stress, EQ.2: Maximum shear stress. NOUT Part, part set, segment set, or node set ID for response output (use with acoustic computation). See NOTYP below. NOTYP Type of NOUT: EQ.0: part set ID (not implemented), EQ.1: part ID (not implemented), EQ.2: segment set ID, EQ.3: node set ID, EQ.-2: segment set ID which mismatches with acoustic boundary nodes. Mapping of velocity or acceleration to the acoustic boundary nodes is performed. NOVA Response output type. EQ.0: velocity, EQ.1: acceleration. RO C Fluid density. Sound speed of the fluid. ERPRLF ERP radiation loss factor. ERPREF ERP reference value. This is used to convert the absolute ERP value to ERP in decibels (dB). VARIABLE PID DESCRIPTION Part, part set, or segment set ID for ERP computation. See PTYP below. PTYP Type of PID: EQ.0: part ID, EQ.1: part set ID, EQ.2: segment set ID. NID Node, node set, or segment set ID for excitation input. See NTYP below. NTYP Type of NID. EQ.0: node ID, EQ.1: node set ID, EQ.2: segment set ID. DOF Applicable degrees-of-freedom for excitation input (ignored if VAD = 1). EQ.1: 𝑥-translational degree-of-freedom, EQ.2: 𝑦-translational degree-of-freedom, EQ.3: 𝑧-translational degree-of-freedom, EQ.4: translational movement in direction given by vector VID. VAD Excitation input type: EQ.0: nodal force, EQ.1: pressure, EQ.2: base velocity, EQ.3: base acceleration, EQ.4: base displacement, EQ.5: enforced velocity by large mass method , EQ.6: enforced acceleration by large mass method , EQ.7: enforced displacement by large mass method . VARIABLE DESCRIPTION Load Curve ID defining amplitude (LCFLAG = 0) or real (in- phase) part (LCFLAG = 1) of load as a function of frequency. Load Curve ID defining phase angle (LCFLAG = 0) or imaginary (out-phase) part (LCFLAG = 1) of load as a function of frequency. Load Curve ID defining load duration for each frequency. This parameter is optional and is only needed for fatigue analysis. Vector ID for DOF = 4 for excitation input, see *DEFINE_VEC- TOR. LC1 LC2 LC3 VID Remarks: 1. This command computes steady state dynamic response due to harmonic excitation spectrum by modal superposition method. 2. Natural frequencies and mode shapes are needed for running the modal superposition method. Thus, the keyword *CONTROL_IMPLICIT_EIGEN- VALUE must be included in input. 3. MDMIN/MDMAX and FNMIN/FNMAX together determine which modes are used in modal superposition method. The first mode must have a mode num- ber ≥ MDMIN, and frequency ≥ FNMIN; The last mode must have mode num- ber ≤ MDMAX, and frequency ≤ FNMAX. When MDMAX or FNMAX is not given, the last mode in modal superposition method is the last mode available in FILENM. 4. Restart option RESTMD = 1 is used if mode analysis has been done previously. In this case, LS-DYNA skips modal analysis and reads in d3eigv family files generated previously. For RESTMD = 1, always use MDMIN = 1 and MDMAX = number of modes given by modal analysis (can be found from ASCII file eigout, or from d3eigv files using LS-PREPOST). 5. Restart option RESTDP = 1 is used if user wants to add contribution of additional modes to previous SSD results. In this case, LS-DYNA reads in bina- ry dump file dumpssd which contains previous SSD results and adds contribu- tion from new modes. For RESTDP = 1, the new modal analysis (RESTMD = 0) or the d3eigv family files created elsewhere (RESTMD = 1) should exclude the modes used in previous SSD computation. This can be done by setting LFLAG (and RFLAG, if necessary), and setting a nonzero LFTEND (and RHTEND) in *CONTROL_IMPLICIT_EIGENVALUE. The RESTDP option can also be used if the frequency range for modal analysis is divided into segments and modal analysis is performed for each frequency range separately. 6. Sometimes customers would like to add some acoustic field nodes and run BEM/FEM acoustic computation after SSD. The RESTMD and RESTDP options still work even if the number of nodes may get changed after previous modal analysis, provided that the IDs of the old nodes are not changed. 7. Damping can be prescribed in several ways: a) To use a constant modal damping coefficient for all the modes, define DAMPF only. LCDMP, LCTYP, DMPMAS and DMPSTF are ignored. b) To use mode dependent modal damping, define a load curve (*DEFINE_- CURVE) and specify that if the abscissa value defines the frequency or mode number by LCTYP. DMPMAS and DMPSTF are ignored. c) To use Rayleigh damping, define DMPMAS (𝛼) and DMPSTF (𝛽) and keep DAMPF as 0.0, and keep LCDMP, LCTYP as 0. The damping matrix in Rayleigh damping is defined as 𝐂 = 𝐌 + 𝐊, where, 𝐂, 𝐌 and 𝐊 are the damping, mass and stiffness matrices respectively. 8. NOUT and NOTYP are used to define the nodes where velocity or acceleration are requested to be written to a binary file “bin_ssd” or other filename defined by “bem=filename” in command line. The velocity or acceleration data in this file can be used by BEM or FEM acoustic solver to perform a vibro-acoustic analysis. If struc- ture nodes and acoustic boundary nodes are mismatched, the option NOTYP = -2 can be used. The velocity or acceleration data given at a structure segment set NOUT is mapped to acoustic boundary nodes. 9. For base velocity, base acceleration or base displacement (VAD = 2, 3 or 4) excitations, the parameters NID, NTYP are not used and can be blank. The base velocity, base acceleration and base displacement cases are treated by applying inertia force to the structure. 10. For the cases with enforced motion excitation such as nodal velocity, accelera- tion, or displacement) the large mass method can be used to compute the SSD results. The excitation input can be given as enforced motion curves (VAD = 5, 6, 7). To use the large mass method, the user need to attach a large mass to the nodes where the enforced motion is applied by using the keyword *ELE- MENT_MASS_{OPTION}, and report the large mass per node (MPN) in the keyword *CONTROL_FREQUENCY_DOMAIN. For more details, please refer to *CONTROL_FREQUENCY_DOMAIN. 11. Displacement, velocity and acceleration results are output into ASCII file NODOUT_SSD. The nodes to be output to NODOUT_SSD are specified by card *DATABASE_HISTORY_NODE. 12. Stress results are output into ASCII file ELOUT_SSD. The solid, beam, shell and thick shell elements to be output to ELOUT_SSD are specified by the fol- lowing cards: *DATABASE_HISTORY_SOLID_{OPTION} *DATABASE_HISTORY_BEAM_{OPTION} *DATABASE_HISTORY_SHELL_{OPTION} *DATABASE_HISTORY_TSHELL_{OPTION} 13. The phase angle is given in range (-180°, 180°]. 14. When the FATIGUE option is present, the cumulative fatigue damage ratio due to the harmonic vibration is computed and saved in binary plot database d3ftg. The *MATERIAL_ADD_FATIGUE keyword is needed to define the S-N fatigue curve for each material. Purpose: Define hourglass and bulk viscosity properties which are referenced via HGID in the *PART command. Properties specified here, when invoked for a particular part, override those in *CONTROL_HOURGLASS and *CONTROL_BULK_VISCOSI- TY. An additional option TITLE may be appended to *HOURGLASS keywords. If this option is used then an additional line is read for each section in 80a format which can be used to describe the section. At present LS-DYNA does not make use of the title. Inclusion of titles gives greater clarity to input decks. Card 1 1 2 3 4 Variable HGID IHQ QM IBQ Type I/A I F I 5 Q1 F 6 7 8 Q2 QB, VDC QW F F F Default 0 .10 1.5 0.06 QM, 0. QM Remark 1,6 2 ,4, 7 3 3 5 5 VARIABLE HGID DESCRIPTION Hourglass ID. A unique number or label must be specified. This ID is referenced by HGID in the *PART command. IHQ DESCRIPTION Hourglass control type. For solid elements six options are available. For quadrilateral shell and membrane elements the hourglass control is based on the formulation of Belytschko and Tsay, i.e., options 1-3 are identical, and options 4-5 are identical: EQ.0: see remark 9, EQ.1: standard LS-DYNA viscous form, EQ.2: Flanagan-Belytschko viscous form, EQ.3: Flanagan-Belytschko viscous form with exact volume integration for solid elements, EQ.4: Flanagan-Belytschko stiffness form, EQ.5: Flanagan-Belytschko stiffness form with exact volume integration for solid elements. EQ.6: Belytschko-Bindeman co- rotational stiffness form for 2D and 3D solid elements only. [1993] assumed strain EQ.7: Linear total strain form of type 6 hourglass control. . EQ.8: Activates full projection warping stiffness for shell formulations 16 and -16, and is the default for these formulations. A speed penalty of 25% is common for this option. EQ.9: Puso [2000] enhanced assumed strain stiffness form for 3D hexahedral elements. EQ.10: Cosserat Point Element (CPE) developed by Jabareen and Rubin [2008] and Jabareen et.al. [2013], see *CON- TROL_HOURGLASS. A discussion of the viscous and stiffness hourglass control for shell elements follows at the end of this section.. Hourglass coefficient. Values of QM that exceed 0.15 may cause instabilities for brick elements used with forms IHG = 0 to 5 and all the IHG forms applicable to shell elements. The stiffness forms can stiffen the response especially if deformations are large and therefore should be used with care. For the shell and membrane elements QM is taken as the membrane hourglass coefficient, the bending as QB, and warping as QW. These coefficients can be specified independently, but generally, QM = QB = QW, is adequate. For type 6 solid element hourglass control, see remark 4 below. For hourglass type 9, see Remark 8. Not used. Bulk viscosity is always on for solids. Bulk viscosity for beams and shells can only be turned on using the variable TYPE the *CONTROL_BULK_VISCOSITY; coefficients can be set using Q1 and Q2 below. however, in Quadratic bulk viscosity coefficient. Linear bulk viscosity coefficient. Hourglass coefficient for shell bending. The default: QB = QM. . Viscous damping coefficient for types 6 and 7 hourglass control. Hourglass coefficient for shell warping. The default: QB = QW. VARIABLE QM IBQ Q1 Q2 QB VDC QW Remarks: 1. Viscous hourglass control is recommended for problems deforming with high velocities. Stiffness control is often preferable for lower velocities, especially if the number of time steps are large. For solid elements the exact volume inte- gration provides some advantage for highly distorted elements. 2. For automotive crash the stiffness form of the hourglass control with a coefficient of 0.05 is preferred by many users. 3. Bulk viscosity is necessary to propagate shock waves in solid materials. Generally, the default values are okay except in problems where pressures are very high, larger values may be desirable. In low density foams, it may be necessary to reduce the viscosity values since the viscous stress can be signifi- cant. It is not advisable to reduce it by more than an order of magnitude. constants and an assumed strain field, it produces accurate coarse mesh bend- ing results for elastic material when QM = 1.0. For plasticity models with a yield stress tangent modulus that is much smaller than the elastic modulus, a smaller value of QM (0.001 to 0.1) may produce better results. For foam or rubber models, larger values (0.5 to 1.0) may work better. For any material, keep in mind that the stiffness is based on the elastic constants, so if the materi- al softens, a QM value smaller than 1.0 may work better. For anisotropic mate- rials, an average of the elastic constants is used. For fluids modeled with null material, type 6 hourglass control is viscous and is scaled to the viscosity coeffi- cient of the material . 5. In part, the computational efficiency of the Belytschko-Lin-Tsay and the under integrated Hughes-Liu shell elements are derived from their use of one-point quadrature in the plane of the element. To suppress the hourglass deformation modes that accompany one-point quadrature, hourglass viscous or stiffness based stresses are added to the physical stresses at the local element level. The discussion of the hourglass control that follows pertains to all one point quadri- lateral shell and membrane elements in LS-DYNA. The hourglass shape vector 𝜏𝐼 is defined as 𝜏𝐼 = ℎ𝐼 − (ℎ𝐽𝑥̂𝑎𝐽)𝐵𝑎𝐼 where, 𝑥̂𝑎𝐽 are the element coordinates in the local system at the Ith element node, 𝐵𝑎𝐼 is the strain displacement matrix, and hourglass basis vector is: ℎ = +1 ⎤ ⎡ −1 ⎥⎥ ⎢⎢ +1 −1⎦ ⎣ is the basis vector that generates the deformation mode that is neglected by one- point quadrature. In the above equations and the remainder of this subsection, the Greek subscripts have a range of 2, e.g., 𝑥̂𝑎𝐼 = (𝑥̂1𝐼 , 𝑥̂2𝐼) = (𝑥̂𝐼 , 𝑦̂𝐼). The hourglass shape vector then operates on the generalized displacements to produce the generalized hourglass strain rates 𝑀 = 𝜏𝐼𝜐̂𝛼𝐼 𝑞 ̇𝛼 𝐵 = 𝜏𝐼𝜃̂ 𝛼𝐼 𝑞 ̇𝛼 𝑊 = 𝜏𝐼𝜐̂𝑧𝐼 𝑞 ̇3 where the superscripts M, B, and W denote membrane, bending, and warping modes, respectively. The corresponding hourglass stress rates are then given by 𝑄̇𝛼 𝑀 = QM × 𝐸𝑡𝐴 𝐵𝛽𝐼𝐵𝛽𝐼𝑞 ̇𝛼 𝐵 = 𝑄̇ 𝑊 = QB × 𝐸𝑡3𝐴 192 QW × 𝜅𝐺𝑡3𝐴 12 𝐵 𝐵𝛽𝐼𝐵𝛽𝐼𝑞 ̇𝛼 𝐵 𝐵𝛽𝐼𝐵𝛽𝐼𝑞 ̇3 where 𝑡 is the shell thickness. The hourglass coefficients: QM, QB, and QW are generally assigned values between 0.05 and 0.10. Finally, the hourglass stresses which are updated using the time step, Δ𝑡, from the stress rates in the usual way, that is, and the hourglass resultant forces are then 𝑸𝑛+1 = 𝑸𝑛 + Δ𝑡𝐐̇ 𝑓 ̂ 𝐻 = 𝜏𝐼𝑄𝛼 𝑀 𝛼𝐼 𝐻 = 𝜏𝐼𝑄𝛼 𝐵 𝑚̂𝛼𝐼 𝑓 ̂ 𝑊 𝐻 = 𝜏𝐼𝑄3 3𝐼 where the superscript H emphasizes that these are internal force contributions from the hourglass deformations. 6. IHQ = 7 is a linear total strain formulation of the Belytschko-Bindeman [1993] stiffness form for 2D and 3D solid elements. This linear form was developed for visco-elastic material and guarantees that an element will spring back to its initial shape regardless of the severity of deformation. 7. The default value for QM is 0.1 unless superseded by a nonzero value of QH in *CONTROL_HOURGLASS. A nonzero value of QM supersedes QH. 8. Hourglass type 9 is available for hexahedral elements and is based on physical stabilization using an enhanced assumed strain method. In performance it is similar to the Belytschko-Bindeman hourglass formulation (type 6) but gives more accurate results for distorted meshes, e.g., for skewed elements. If QM = 1.0, it produces accurate coarse bending results for elastic materials. The hourglass stiffness is by default based on elastic properties, hence the QM pa- rameter should be reduced to about 0.1 for plastic materials in order not to stiffen the structure during plastic deformation. For materials 3, 18 and 24 there is the option to use a negative value of QM. With this option, the hourglass stiffness is based on the current material properties, i.e., the plastic tangent modulus, and scaled by ∣QM∣. 9. The default value for IHQ, if not defined on *CONTROL_HOUGRGLASS is as follows: For shells: viscous type (1 = 2 = 3) for explicit; stiffness type (4=5) for implicit For formulation 1 tshells: type 2. 10. For implicit analysis, hourglass forms 6, 7, 9, and 10 are available for solid elements, and the stiffness form (4 = 5) is available for shells. 11. Tshell formulations 2 and 3 have 2 × 2 in-plane integration and therefore do not use hourglass control. 12. In the case of tshell formulation 1, there are two viscous hourglass types (IHQ = 1,2) and one stiffness type (IHQ > 2). 13. The hourglass type IHQ has no bearing on tshell formulation 5 as this formulation is based on an assumed strain field, similar to formulation 1 solids with hourglass type 6. The hourglass coefficient QM does affect the behavior of tshell formulation 5. Purpose: The keyword *INCLUDE provides a means of reading independent input files containing model data. The file contents are placed directly at the location of the *INCLUDE line. *INCLUDE_{OPTION} *INCLUDE_AUTO_OFFSET *INCLUDE_COMPENSATION_OPTION *INCLUDE_MULTISCALE_SPOTWELD *INCLUDE_TRIM *INCLUDE_UNITCELL *INCLUDE_{OPTION} Available options include: <BLANK> BINARY NASTRAN PATH PATH_RELATIVE STAMPED_SET TRANSFORM TRANSFORM_BINARY STAMPED_PART_{OPTION1}_{OPTION2}_{OPTION3} OPTION1: SET OPTION2: MATRIX OPTION3: INVERSE The BINARY and TRANSFORM_BINARY options specify that the initial stress file, dynain, is written in a binary format. See the keyword *INTERFACE_SPRINGBACK. The PATH option defines a directory in which to look for the include files. The program always searches the local directory first. If an include file is not found and the filename has no path, the program will search for it in all the directories defined by *IN- CLUDE_PATH. Multiple paths can defined with one *INCLUDE_PATH definition, i.e., *INCLUDE_PATH Directory_path1 Directory_path2 Directory_path3 Directory paths are read until the next “*” card is encountered. A directory path can have up to 236 characters . The PATH_RELATIVE option is like the PATH option, except all directories are relative to the location of the input file. For example, if “i=/home/test/problems/input.k” is given on the command line, and the input contains *INCLUDE_PATH_RELATIVE Includes ../includes then the two directories /home/test/problems/includes and /home/test/includes will be searched for include files. The STAMPED_PART option applies only to thin shell elements and allows the plastic strain and thickness distribution of the stamping simulation to be mapped onto a part in the crash model. 1. When option 1, SET is used, the PID will be part set ID. All the parts included in this set will be considered in this mapping. 2. When option 2, MATRIX is used, translation matrix will be read directly and the orientation nodes will be ignored. 3. When option 3, INVERSE (must be used with MATRIX) is used, the matrix will be reversed first. When STAMPED_SET is used, the target is a part set ID. Between the stamped part and the crash part, note the following points: 1. The outer boundaries of the parts do not need to match since only the regions of the crash part which overlap the stamped part are initialized. 2. Arbitrary mesh patterns are assumed. 3. Element formulations can change. 4. Three nodes on each part are used to reorient the stamped part for the mapping of the strain and thickness distributions. After reorientation, the three nodes on each part should approximately coincide. 5. The number of in plane integrations points can change. 6. The number of through thickness integration points can change. Full interpola- tion is used. 7. The node and element ID's between the stamped part and the crash part do not need to be unique. The TRANSFORM option allows for node, element, and set ID's to be offset and for coordinates and constitutive parameters to be transformed and scaled. Card 1 1 2 3 4 5 6 7 8 Variable Type FILENAME C If the *INCLUDE command is used without options, multiple filenames can be specified, i.e., *INCLUDE Filename1 Filename2 Filename3 which are processed sequentially. Filenames are read until the next “*” card is encountered. Nastran Card. Additional Card for the NASTRAN keyword option. Card 2 1 2 3 4 5 6 7 8 Variable BEAMDF SHELLDF SOLIDDF Type Default I 2 I I 21 18 Stamped Part Card 1. Additional Card for STAMPED_PART keyword option. Card 2 1 2 3 4 5 6 7 8 Variable PID THICK PSTRN STRAIN STRESS INCOUT RMAX Type I Default none I 0 I 0 I 0 I 0 I 0 F 20.0 Stamped Part Card 2a. Additional card for STAMPED_PART option not ending in_ MATRIX. Card 3 1 2 3 4 5 6 7 8 Variable N1S N2S N3S N1C N2C N3C TENSOR THKSCL Type Default Remarks I 0 2 I 0 2 I 0 2 I 0 2 I 0 2 I 0 2 I 0 4 F 1.0 Stamped Part (Matrix) Card 2b. Additional card for STAMPED_PART_MATRIX option. 5 6 7 8 Card 3 1 2 3 Variable R11 R12 R13 Type Default Remarks F 0 2 F 0 2 F 0 2 4 XP F 0 2 Stamped Part (Matrix) Card 3. Additional card for STAMPED_PART_MATRIX option. Card 4 1 2 3 Variable R21 R22 R23 Type Default Remarks F 0 2 LS-DYNA R10.0 F 0 2 F 0 2 4 YP F 0 2 5 6 Stamped Part (Matrix) Card 4. Additional card for STAMPED_PART_MATRIX option. 5 6 7 8 Card 5 1 2 3 Variable R31 R32 R33 Type Default Remarks F 0 2 F 0 2 F 0 2 4 ZP F 0 2 Remaining Stamped Part cards are optional.† Stamped Part Card 6. Optional card for STAMPED_PART (with and without_MA- TRIX) keyword option. Card 4 1 2 3 4 5 6 7 8 Variable ISYM IAFTER PERCELE IORTHO ISRCOUT Type I I F I I Stamped Part Card 6. Optional card for STAMPED_PART (with and without_MA- TRIX) keyword option. Card 5 1 2 3 4 5 6 7 8 Variable X01 Y01 Z01 Type F F Stamped Part Card 7. Optional card for STAMPED_PART (with and without_MA- TRIX) keyword option. Card 6 1 2 3 4 5 6 7 8 Variable X02 Y02 Z02 X03 Y03 Z03 Type F F F F F F Transform Card 1. Additional card for TRANSFORM keyword option. Card 2 1 2 3 4 5 6 7 8 Variable IDNOFF IDEOFF IDPOFF IDMOFF IDSOFF IDFOFF IDDOFF Type I I I I I I I Transform Card 2. Additional card for TRANSFORM keyword option. Card 3 1 2 3 4 5 6 7 8 Variable IDROFF PREFIX SUFFIX Type I A A Transform Card 3. Additional card for TRANSFORM keyword option. Card 4 1 2 3 4 5 6 7 8 Variable FCTMAS FCTTIM FCTLEN FCTTEM INCOUT1 Type F F F A Transform Card 4. Additional card for TRANSFORM keyword option. Card 5 1 2 3 4 5 6 7 8 Variable TRANID Type Default I 0 VARIABLE FILENAME DESCRIPTION File name of file to be included in this keyword file, 80 characters maximum. If the STAMPED_PART option is active, this is the dynain file containing the results from metal stamping. BEAMDF LS-DYNA beam element type. Defaults to type 2. SHELLDF LS-DYNA shell element type. Defaults to type 21. SOLIDDF LS-DYNA solid element type. Defaults to type 18. PID Part ID of crash part for remapping. THICK Thickness remap: EQ.0: map thickness EQ.1: do not map thickness EQ.2: average value inside a circle defined by RMAX PSTRN Plastic strain remap: EQ.0: map plastic strain EQ.1: do not plastic strain EQ.2: average value inside a circle defined by RMAX STRAIN Strain remap: EQ.0: map strains EQ.1: do not map strains VARIABLE DESCRIPTION STRESS Stress tensor remap: EQ.0: map stress tensor and history variables EQ.1: do not map stress tensor, only history variables EQ.2: neither map stress tensor nor history variables EQ.-1: map stress tensor in an internal large format (binary files) EQ.-3: do not map stress tensor in an internal large format, only history (binary files) EQ.1: to save the mapped data to a file called dyna.inc, which contains the mapped data for the part that is being mapped. This option is useful to do mapping using IN- CLUDE_STAMPED_PART and then save the mapped data for future use. When INCOUT is set to 2, the output file is in dynain format and the file name is dynain_xx (xx is the part or part set id); and when INCOUT is set to 3, the output file is in NASTRAN format, and the file name is: nastran_xx. EQ.2: to save the mapped data for the specified part (PID) to a file called dynain_PID. EQ.3: to save the mapped data for the specified part (PID) to a file called nastran_PID (in nastran format) Search radius. LS-DYNA remaps history variables from the mesh of the stamped part to the mesh of the crash part with a spatial tolerance of RMAX. If an element in the crash part lies within RMAX of the stamped part, data will be mapped to that element. If set less than 0.001, RMAX automatically assumes the default value of 20. First of 3 nodes needed to reorient the stamped part. Second of 3 nodes needed to reorient the stamped part. Third of 3 nodes needed to reorient the stamped part. First of 3 nodes needed to reorient the crash model part. Second of 3 nodes needed to reorient the crash model part. Third of 3 nodes needed to reorient the crash model part. INCOUT RMAX N1S N2S N3S N1C N2C N3C VARIABLE DESCRIPTION TENSOR Tensor remap: EQ.0: map tensor data from history variables. EQ.1: do not map tensor data from history variables THKSCL Thickness scale factor. R11, R12, R33 Components of the transformation matrix. XP, YP, ZP Translational distance. ISYM Symmetric switch EQ.0: no symmetric mapping EQ.1: 𝑦𝑧 plane symmetric mapping EQ.2: 𝑧𝑥 plane symmetric mapping EQ.3: 𝑧𝑥 and 𝑦𝑧 planes symmetric mapping EQ.4: user defined symmetric plane mapping IAFTER Mirroring sequence switch EQ.0: generate a symmetric part before transformation EQ.1: generate a symmetric part after transformation PERCELE Percentage of elements that should be mapped to proceed (default = 0); otherwise an error termination occurs. See Remark 6. IORTHO Location of the material direction cosine in the array of history variables of an orthotropic material. See Remark 5. ISRCOUT Optional output of stamped part after transformation(s) EQ.0: no output is written NE.0: keyword output file “srcmsh_<ISRCOUT>” is created X01, Y01, Z01 First point in the symmetric plane (required if ISYM.NE.0) X02, Y02, Z02 Second point in the symmetric plane X03, Y03, Z03 Third point in the symmetric plane IDNOFF Offset to node ID. VARIABLE DESCRIPTION IDEOFF Offset to element ID. IDPOFF Offset to part ID, nodal rigid body ID, constrained nodal set ID, Rigidwall ID, and *DATABASE_CROSS_SECTION. IDMOFF Offset to material ID and equation of state ID. IDSOFF Offset to set ID. IDFOFF Offset to function ID, table ID, and curve ID. IDDOFF to any Offset FUNCTION, TABLE, and CURVE options . through *DEFINE except ID defined the IDROFF Used for all offsets except for those listed above. PREFIX SUFFIX FCTMAS FCTTIM Prefix added to the beginning of the titles/heads defined in the keywords for examples) of the included file. A dot, “.”, is automatically added between the prefix and the existing title. (like *MAT, *PART, *SECTION, *DEFINE, Suffix added to the end of the titles/heads defined in the keywords of the included file. A dot, “.”, is automatically added between the suffix and the existing title. Mass transformation factor. When the original mass units are in tons and the new unit is kg. For example, FCTMAS = 1000. Time transformation factor. For example, FCTTIM=.001 when the original time units are in milliseconds and the new time unit is seconds. FCTLEN Length transformation factor. FCTTEM INCOUT1 Temperature transformation factor consisting of a four character flag: FtoC (Fahrenheit to Centigrade), CtoF, FtoK, KtoF, KtoC, and CtoK. Set to 1 for the creation of a file, DYNA.INC, which contains the transformed data. The data in this file can be used in future include files and should be checked to ensure that all the data was transformed correctly. TRANID Transformation ID, if 0 no transformation will be applied. See the input DEFINE_TRANSFORMATION. *INCLUDE_{OPTION} 1. Scalability. To make the input file easy to maintain, this keyword allows the input file to be split into subfiles. Each subfile can again be split into sub- subfiles and so on. This option is beneficial when the input data deck is very large. Consider the following example: *TITLE full car model *INCLUDE carfront.k *INCLUDE carback.k *INCLUDE occupantcompartment.k *INCLUDE dummy.k *INCLUDE bag.k *CONTACT ⋮ *END Note that the command *END terminates the include file. The carfront.k file can again be subdivided into rightrail.k, leftrail.k, battery.k, wheel-house.k, shotgun.k, etc.. Each *.k file can include nodes, elements, boundary conditions, initial conditions, and so on. *INCLUDE rightrail.k *INCLUDE leftrail.k *INCLUDE battery.k *INCLUDE wheelhouse.k *INCLUDE shotgun.k ⋮ *END 2. Reorienting the Result of a Stamping Simulation for STAMPED_PART option. When defining *INCLUDE_STAMPED_PART the target mesh must be read in before the include stamped part. N1S, N2S, N3S, N1C, N2C, and N3C are used for transforming the stamped part to the crash part, such that it is in the same position as the crash part. If the stamped part is in the same position as the crash part then N1S, N2S, N3S, N1C, N2C, N3C can all be set to 0. Note: If these 6 nodes are input as 0, LS-DYNA will not transform the stamped part. When symmetric mapping is used (ISYM is not zero), the three points should not be in one line. If ISYM = 0, 1, 2, or 3, only the first point (X01,Y01, Z01) is needed If ISYM = 4, all the three points are needed 3. Path Length Limitations. Filenames and pathnames are limited to 236 characters spread over up to three 80 character lines. When 2 or 3 lines are needed to specify the filename or pathname, end the preceding line with "˽+" (space followed by a plus sign) to signal that a continuation line follows. Note that the "˽+" combination is, itself, part of the 80 character line; hence the maxi- mum number of allowed characters is 78 + 78 + 80 = 236. 4. Mapping Material Data for Springback for STAMPED_PART option. Certain material models (notably Material 190) have tensor data stored within the history variables. Within material subroutines this data is typically stored in element local coordinate systems. In order to properly map this information between models it is necessary to have the tensor data present on the *INI- TIAL_STRESS_SHELL card and have it stored in global coordinates. During mapping the data is then converted into the local coordinate system of the crash mesh. This data can be dumped into the dynain file that is created at termina- tion time if the parameter FTENSR is set to 0 on the *INTERFACE_SPRING- BACK_DYNA3D card. Currently, the only material model that supports mapping of element history tensor data is Material 190. 5. IORTHO. If IORTHO is set, correct mapping between non-matching meshes is invoked for the directions of orthotropic materials. A list of appropriate values for several materials is given here: IORTHO.EQ.1: materials 23, 122, 157, 234 IORTHO.EQ.3: materials 22, 33, 36, 133, 189, 233, 243 IORTHO.EQ.4: material 59 IORTHO.EQ.6: materials 58, 104, 158 IORTHO.EQ.8: materials 54, 55 IORTHO.EQ.9: material 39 IORTHO.EQ.10: material 82 IORTHO.EQ.13: materials 2, 86, 103 6. Mapping Mismatch with STAMPED_PART option. Sometimes during mapping the two meshes (stamp mesh and crash mesh) do not fit exactly and therefore not all elements of the new mesh get results from the old mesh. In- formation about the total number of crash elements which are / are not mapped is given in the message file. By default (PERCELE=0), the calculation continues even with zero number of mapped elements. With PERCELE>0 the percentage of minimum number of elements can be defined, which have to be mapped. If a percentage less than PERCELE is mapped, calculation stops with an error termination. 7. NASTRAN Option. The transformed LS-Dyna deck for *INCLUDE_NASTRAN will be automatically written to file DYNA.INC. *INCLUDE Purpose: This particular *INCLUDE keyword offsets node and element IDs to avoid duplication during stamping simulations. In stamping simulations the rigid tools often undergo several iterations of modifications. The node or element IDs comprising the new tools sometimes conflict with other parts of the model, which makes it difficult to automate the process simulation. This keyword automatically checks for and fixes duplicate IDs. The *CONTROL_FORMING_MAXID keyword is related. Card 1 1 2 3 4 5 6 7 8 Variable Type FILENAME C VARIABLE DESCRIPTION FILENAME File name to be included. Remarks: This keyword can be used to offset element and node IDs of the tooling. The keyword will not offset meshes with initial stress and strain information. As such, sheet blank (including dynain file) should always be included first using the *INCLUDE keyword, followed by *INCLUDE_AUTO_OFFSET to offset tooling mesh IDs which do not have stress and strain information. Incoming element and node IDs of the tooling mesh files such as the punch, die, and binder, can be overlapped with each other, or overlapped with those on the sheet blank. Multiple *INCLUDE_AUTO_OFFSET can be used to include punch, die, binder separately, if desired. For example, four different components of the tooling, upper die, lower punch, binder and gage pins can be included and their element and node IDs properly offset after those of a gravity-loaded sheet blank: *INCLUDE gravity.dynain *INCLUDE_AUTO_OFFSET upperdie.k *INCLUDE_AUTO_OFFSET lowerpunch.k *INCLUDE_AUTO_OFFSET binder.k *INCLUDE_AUTO_OFFSET pins.k All of the included meshes can have conflicting mesh IDs starting from “1”. Mesh IDs will be offset and reordered in the order of the tool inclusion using *INCLUDE_AU- TO_OFFSET. Included tool files whose mesh IDs do not overlap with those on either the blank or other tools will not be offset or reordered. In many circumstances this feature allows the user to bypass the metal forming GUI when updating just one or two tooling pieces. Revision information: This feature is available in SMP and MPP starting in LS-DYNA Revision 92417. Revision 117818 extends the keyword to beams (used to model draw beads, for example) and solids. *INCLUDE_COMPENSATION_{OPTION} Purpose: This group of keywords allow for the inclusion of stamping die geometry information for springback compensation. In addition, trim curves from the target geometry can be included for mapping onto the intermediate compensated tool geometry, which can be used for the next compensation iteration. Furthermore, compensation can be done for a localized tool region. These keywords must be used together with *INTERFACE_COMPENSATION_NEW. Options available include: BLANK_BEFORE_SPRINGBACK BLANK_AFTER_SPRINGBACK DESIRED_BLANK_SHAPE COMPENSATED_SHAPE CURRENT_TOOLS TRIM_CURVE CURVE ORIGINAL_DYNAIN SPRINGBACK_INPUT COMPENSATED_SHAPE_NEXT_STEP SYMMETRIC_LINES ORIGINAL_RIGID_TOOL NEW_RIGID_TOOL ORIGINAL_TOOL UPDATED_BLANK_SHAPE UPDATED_RIGID_TOOL Blank Before Springback Card. Additional card for BLANK_BEFORE_SPRING- BACK keyword option. Card 1 1 2 3 4 5 6 7 8 Variable Type Default FILENAME C blank0.tmp Blank After Springback Card. Additional card for BLANK_AFTER_SPRINGBACK keyword option. Card 1 1 2 3 4 5 6 7 8 Variable Type Default FILENAME C spbk.tmp Desired Blank Shape Card. Additional card for DESIRED_BLANK_SHAPE keyword option. Card 1 1 2 3 4 5 6 7 8 Variable Type Default FILENAME C reference0.dat Compensated Shape Card. Additional card for COMPENSATED_SHAPE keyword option. Card 1 1 2 3 4 5 6 7 8 Variable Type Default FILENAME C reference1.dat Current Tools Card. Additional card for CURRENT_TOOLS keyword option. Card 1 1 2 3 4 5 6 7 8 Variable Type Default FILENAME C rigid.tmp Generic Filename Card. Additional Card for TRIM_CURVE, CURVE, ORIGINAL_- DYNAIN, SPRINGBACK_INPUT, COMPENSATED_SHAPE_NEXT_STEP, ORIGI- NAL_RIGID_TOOL, NEW_RIGID_TOOL, ORIGINAL_TOOL, UPDATED_BLANK_- SHAPE, and UPDATED_RIGID_TOOL keyword options. Card 1 1 2 3 4 5 6 7 8 Variable Type Default FILENAME C See Remarks Symmetric Lines Cards. Additional card for SYMMETRIC_LINES keyword option. Card 1 1 2 Variable SYMID SYMXY 5 6 7 8 3 X0 F 4 Y0 F I Type Default I 1 VARIABLE FILENAME none 0.0 0.0 DESCRIPTION For options below, input the name of the keyword files containing nodes and elements information, with adaptive constraints if exist. Currently all sheet blanks must have the same numbers of nodes and elements. BLANK_BEFORE_SPRINGBACK, BLANK_AFTER_SPRINGBACK, DESIRED_BLANK_SHAPE, COMPENSATED_SHAPE, CURRENT_TOOLS, COMPENSATED_SHAPE_NEXT_STEP For option ORIGINAL_DYNAIN, input the dynain file name from LS-DYNA simulation (for example, trimmed panel from ITER0 baseline simulation) which contains model information, adaptive constraints, stress and strain tensor information. This keyword is to be used in conjunction with *INTERFACE_COM- PENSATION_NEW_ACCELATOR. the file name of For option SPRINGBACK_INPUT, give springback simulation input deck for the baseline ITER0 simulation. This keyword is to be used in conjunction with *IN- TERFACE_COMPENSATION_NEW_ACCELATOR. For option TRIM_CURVE, input the name of the keyword file containing 𝑥, 𝑦, 𝑧 coordinates as defined using keyword *DE- FINE_CURVE_TRIM_3D (only TCTYPE = 0, or 1 is supported). This option is used to map the trim curve to the new, VARIABLE DESCRIPTION compensated tooling mesh for next iterative simulation. For option CURVE, input the name of the keyword file containing 𝑥, 𝑦, 𝑧 coordinates of two curves defining the compensation zone, using keywords: *DEFINE_CURVE_COMPENSATION_CON- STRAINT_BEGIN, and, *DEFINE_CURVE_COMPENSATION_- CONSTRAINT_END. This option is for compensation of localized tooling areas. All foregoing keyword options are used together with *INTER- FACE_COMPENSATION_NEW. For options ORIGINAL_RIGID_TOOL and NEW_RIGID_TOOL, input the file names of the keyword file containing meshes of the rigid tools. This option is used to smooth distorted meshes of localized tool surfaces. These keyword options are used together with *INTERFACE_COMPENSATION_NEW_LOCAL_- SMOOTH. For option ORIGINAL_TOOL, input the file name of the original tool (without any compensation) mesh containing nodes and elements information in keyword format. This option allow the use of the original tool mesh, which is of higher quality, in the iterative compensation runs, to minimize the tool surface mesh distortion in the addendum and binder areas of the compensated tool . These keyword options are used together with *INTERFACE_COMPENSATION_NEW. For options UPDATED_BLANK_SHAPE, and UPDATED_- RIGID_TOOL, input the respective mesh information in keyword format. The updated blank shape is the blank formed (or trimmed) shape based on the new tool (die) geometry. These options allow for updating of compensated tool shape for small part shape changes, without the need to go through a full-blown iterative compensation loop again . The options are used together with *INTERFACE_COMPENSATION_NEW_- PART_CHANGE, among others. SYMID ID of the symmetric condition being defined. VARIABLE DESCRIPTION SYMXY Code defining symmetric boundary conditions: EQ.1: symmetric about 𝑦-axis. EQ.2: symmetric about 𝑥-axis. X0, Y0 Coordinates of a point on the symmetric plane. Default Filenames: Keyword Option Default Filename UPDATED_BLANK_SHAPE updatedpart.tmp UPDATED_RIGID_TOOL newrigid.tmp About various options: This group of keywords is used in conjunction with *INTERFACE_COMPENSATION_- NEW, to compensate stamping tool shapes for springback with an iterative method. The method approaches the final target design intent from two opposite directions from iteration to iteration. A typical successful compensation requires about 3 to 4 iterations. 1. BLANK_BEFORE_SPRINGBACK. When the option BLANK_BEFORE_- SPRINGBACK is used, the included file is the mesh information in keyword format in the first state (from d3plot) of the springback simulation, or the “dynain” file after trimming (before springback and with no mesh coarsening). The default file name is “blank0.tmp”. 2. BLANK_AFTER_SPRINBACK. When the option BLANK_AFTER_SPRIN- BACK is used, the included file is the “dynain” file after springback, or the last state mesh (from d3plot) of the springback. The default file name is “spbk.tmp”. 3. DESIRED_BLANK_SHAPE. When the option DESIRED_BLANK_SHAPE is used, the included file is the “dynain” file after trimming in the first iteration. This file never changes in all subsequent iterative compensation. The file name default is “reference0.dat”. 4. COMPENSATED_SHAPE. When the option COMPENSATED_SHAPE is used, the included file for the first iteration, is a “dynain” file, same as in the option DESIRED_BLANK_SHAPE; and for the following compensation iterations, this file is obtained from the file “disp.tmp” generated as an output file during the previous compensation iteration. The default file name is “reference1.dat”. 5. CURRENT_TOOLS. When the option CURRENT_TOOLS is used, the included file is the file containing the tool mesh in the keyword format. This is the tool mesh from the last compensation run and used for the current forming simula- tion. The draw bead nodes have to be included in this file so that they will be modified together with the rigid tools. The default file name is “rigid.tmp”, and if the file is named as “rigid0.tmp” the elements of the tools get refined along the outline of the part. 6. TRIM_CURVE. When the option TRIM_CURVE is used, trim curves off the current tools are mapped onto the compensated tools for the trimming opera- tion in the next iteration. If the trimming simulation uses the IGES format trim curves, a new file “geo- cur.trm” will be generated at the end of the trimming simulation. The file basi- cally contains XYZ data of the trim curves in keyword *DEFINE_CURVE_- TRIM_{OPTIONS}, which is used for the compensation run. Note that the variable TCTYPE in the keyword must be set to “0” (or “1”) for the compensa- tion. Length of lines everywhere in the compensated part are calculated ac- cording to springback amounts (including the die expansion factors, therefore no die expansion needs to be included in the NC machining of the compensated tooling). These mapped trim curves can be used for die development on the compensated tools and for laser trimming of stamped panels. Procedures out- line in keyword manual pages *INTERFACE_BLANKSIZE can be followed to convert in LS-PrePost IGES file of the trim curves to XYZ format (and vice ver- sa) used in this keyword. In an example keyword input shown below, the file name for this option is trimcurves.k. The format is in XYZ format, written with LS-PrePost: *DEFINE_CURVE_TRIM_3D $# tcid tctype tflg tdir tctol toln nseed 1116 1 1 0.100 1 $# cx cy cz 178.05170 -326.24771 51.924496 177.77397 -301.90869 50.288792 177.29764 -265.39716 48.594341 ... 7. CURVE. When the option CURVE is used, it allows for die face compensation of a local region in a stamping die. This option is used in conjunction with two more keywords defining two enclosed curves that form the compensation zone in position coordinates 𝑥, 𝑦, 𝑧: *DEFINE_CURVE_COMPENSATION_CON- STRAINT_BEGIN, *DEFINE_CURVE_COMPENSATION_CON- STRAINT_END. Detailed usage of these two keywords is available in the related manual pages. and *INCLUDE_COMPENSATION The following example is for compensation of a localized area, defined by the file curves.k. Trim lines are mapped onto the new compensated rigid tool, with trimcurves.k. Both files which were generated by LS-PrePost 4.0 are in the “XYZ format”. A detailed explanation of each keyword is given in the manual pages related to *INTERFACE_COMPENSATION_NEW. *KEYWORD $---+----1----+----2----+----3----+----4----+----5----+----6----+----7----+-- *INTERFACE_COMPENSATION_NEW $ METHOD SL SF ELREF PSID UNDRCT ANGLE NLINEAR 8 10.000 1.000 0 1 0 0.0 1 *INCLUDE_COMPENSATION_BLANK_BEFORE_SPRINGBACK blank0.k *INCLUDE_COMPENSATION_BLANK_AFTER_SPRINGBACK spbk.k *INCLUDE_COMPENSATION_DESIRED_BLANK_SHAPE reference0.k *INCLUDE_COMPENSATION_COMPENSATED_SHAPE reference1.k *INCLUDE_COMPENSATION_CURRENT_TOOLS tools.k *INCLUDE_COMPENSATION_TRIM_CURVE trimcurves.k $$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ $ For compensation of a localize region only, add the following keyword: *INCLUDE_COMPENSATION_CURVE curves.k $$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ *SET_PART_LIST $ PSID 1 $ PID 3 $---+----1----+----2----+----3----+----4----+----5----+----6----+----7----+-- *END The option ORIGINAL_DYNAIN and SPRINGBACK_INPUT are used together with keyword *INTERFACE_COMPENSATION_NEW_ACCELATOR, for a springback compensation with a faster convergence rate and a simplified user interface. For detailed usage, please refer to manual pages under *INTERFACE_COMPEN- STION_{OPTION}. Here a complete keyword input is provided: *KEYWORD *INTERFACE_COMPENSATION_NEW_ACCELATOR $ ISTEPS TOLX TOLY TOLZ OPTION 3 0.20 0.20 0.2 1 *INCLUDE_COMPENSATION_ORIGINAL_DYNAIN ./case20trimmed.dynain *INCLUDE_COMPENSATION_SPRINGBACK_INPUT ./spbk.dyn *END The option COMPENSATED_SHAPE_NEXT_STEP enables compensation of tools for the next die process. It is used in conjunction with keyword *INTERFACE_COMPEN- SATION_NEW_MULTI_STEPS, which is discussed in the corresponding manual pages. Here a complete input deck is given below: *KEYWORD *INTERFACE_COMPENSATION_NEW_MULTI_STEPS $---+----1----+----2----+----3----+----4----+----5----+----6----+----7----+----8 $ METHOD SL SF ELREF PSID UNDRCT ANGLE NLINEAR 8 6.000 1.00 1 1 0 0 1 *INCLUDE_COMPENSATION_DESIRED_BLANK_SHAPE reference0.tmp *INCLUDE_COMPENSATION_COMPENSATED_SHAPE_NEXT_STEP Reference1_flanging.tmp *INCLUDE_COMPENSATION_CURRENT_TOOLS rigid.tmp *SET_PART_LIST $ PSID 1 $ PID 2 *END The option SYMMTRIC_LINES applies to compensation Method 7 and 8, as discussed in *INTERFACE_COMPENSATION_NEW. In a complete keyword input example below, part set ID 1 is being compensated with symmetric boundary condition about X- axis. The symmetric plane passes a point with coordinates of x = 101.5, and y = 0.0. *KEYWORD $---+----1----+----2----+----3----+----4----+----5----+----6----+----7----+----8 $*INTERFACE_COMPENSATION_NEW $ Method = 8 changes the binder; Method = 7 binder/P.O. no changes. *INTERFACE_COMPENSATION_NEW $ METHOD SL SF ELREF PSID UNDRCT ANGLE NLINEAR 7 10.000 1.000 2 1 1 0.0 1 *INCLUDE_COMPENSATION_BLANK_BEFORE_SPRINGBACK ./state1.k *INCLUDE_COMPENSATION_BLANK_AFTER_SPRINGBACK ./state2.k *INCLUDE_COMPENSATION_DESIRED_BLANK_SHAPE ./state1.k *INCLUDE_COMPENSATION_COMPENSATED_SHAPE ./state1.k *INCLUDE_COMPENSATION_CURRENT_TOOLS ./currenttools.k *INCLUDE_COMPENSATION_SYMMETRIC_LINES $ SYMID SYMXY X0 Y0 1 2 101.5 0.0 $ SYMXY = 2: symmetric about X-axis *SET_PART_LIST $ PSID 1 $ PID 1 *END The options ORIGINAL_RIGID_TOOL and NEW_RIGID_TOOL are used together with *INTERFACE_COMPENSATION_NEW_LOCAL_SMOOTH, and *SET_NODE_LIST_- SMOOTH, to smooth local areas of distorted meshes of a tooling surface. Details can be found *INTERFACE_COMPENSATION_NEW_LOCAL_- SMOOTH. in manual pages for The option ORIGINAL_TOOL is used to obtain a smoother mesh for the addendum and binder region for the current compensation, using the original tool mesh (of better quality) instead of the last compensated tool mesh (maybe distorted). This reduces the accumulative error in mesh extrapolation outside of the trim lines. Details can be found in manual pages for *INTERFACE_COMPENSATION_NEW. The options UPDATED_BLANK_SHAPE, and UPDATED_RIGID_TOOL calculate a new compensated tool shape according to the updated blank shape, thus eliminating the need to go through a full-blown iterative compensation loop again. Note that these options are intended only for small part changes that do not substantially affect the amount of springback. More details can be found in manual pages for *INTERFACE_- COMPENSATION_NEW_PART_CHANGE. Revision information: The option TRIM_CURVE is available starting in Revision 60398. The options ORIGI- NAL_DYNAIN, and SPRINGBACK_INPUT are available starting in Revision 61264. The option COMPENSATED_SHAPE_NEXT_STEP is available starting in Revision 61406. The option CURVE is available starting in Revision 62038. The option SYM- METRIC_LINES is available starting in Revision 63618 (updated in Rev. 83711). The options of ORIGINAL_RIGID_TOOL and NEW_RIGID_TOOL are available starting in Revision 73850. The option ORIGINAL_TOOL is available starting in Revision 82701. The options UPDATED_BLANK_SHAPE, and UPDATED_RIGID_TOOL are available starting in Revision 82698. . *INCLUDE_MULTISCALE_SPOTWELD Purpose: To define a type of MULTISCALE spot weld to be used for coupling and for modeling of spot weld failure. Card 1 1 2 3 4 5 6 7 8 Variable TYPE Type I Default none Card 2 1 2 3 4 5 6 7 8 Variable Type Default VARIABLE TYPE FILENAME C none DESCRIPTION TYPE for this multiscale spot weld. This type is used in the keyword *DEFINE_SPOTWELD_MULTISCALE. Any unique integer will do. FILENAME Name of file from which to read the spot weld definition. Remarks: This capability is available only in the MPP version of LS-DYNA. With the multiscale spot weld feature heuristic spot weld models are replaced with zoomed-in geometrically and constitutively correct continuum models, which, in turn are coupled to the large-scale calculation without reducing the time step. In some respects, multiscale models are similar to the “hex spot weld assemblies,” capability but more general in terms of their geometry. Because the spot weld models are run in a separate process, they can run at a much smaller time step without slowing down the rest of the simulation. A brief outline of their use looks like this: • The user creates one (or more) detailed models of their spot welds, and includes these definitions into their model using the keyword *INCLUDE_MULTI- SCALE_SPOTWELD • The user indicates which beam (or hex assembly) spot welds should be coupled to these models via the keyword *DEFINE_SPOTWELD_MULTISCALE • When MPP-DYNA is started, a special (MPI dependent) invocation is required in order to run in a “multiple program” mode. Effectively, two separate instances of MPP-DYNA are started together, one to run the full model and a separate instance to run the spot welds. • As the master process runs, each cycle it communicates to the slave process deformation information for the area surrounding each coupled spot weld. The slave process imposes this deformation on the detailed spot welds, computes a failure flag for each, and communicates this back to the master process. • The coupled spot welds in the master process have their failure determined solely by these failure flags. The file referred to on the *INCLUDE_MULTISCALE_SPOTWELD card should contain one generic instance of a detailed spot weld. For each coupled spot weld in the main model, a specific instance of this spot weld will be generated which is translated, rotated, and scaled to match the spot weld to which it is coupled. In this way, many spot welds can be coupled with only a single *INCLUDE_MULTISCALE_SPOTWELD. The included file should contain everything required to define the spot weld, such as *MAT and *PART definitions, any required *DEFINE_CURVEs, etc., as well as *NODE and *ELEMENT definitions. In order for the translation and scaling to work properly there are some assumptions made about the spot weld model: • It consists entirely of solid elements. • The 𝑧-axis is aligned with the coupled spot weld in the main model, with 𝑧 = 0 and 𝑧 = 1 at the two ends of the spot weld. • The cross sectional area of the spot weld in the 𝑥𝑦 plane is equal to 1. • That portion of the “top” and “bottom” of the spot weld that are coupled are identified using a single *SET_NODE_LIST card. • One *BOUNDARY_COUPLED card referencing the *SET_NODE_LIST of the boundary nodes is required. It must specify a coupling type of 2 and a coupling program of 1. • The spot weld model does not support *INCLUDE cards. Failure of the fine model is determined topologically. Any element of the spot weld having all four nodes of one of its faces belonging to the *SET_NODE_LIST of tied nodes is classified as a “tied” element. The “tied” elements are partitioned into two disjoint sets: the “top,” and “bottom”. When there is no longer a complete path from any “top” to any “bottom” element (where a “path” passes through non-failed elements that share a common face), then the spot weld has failed. Note that this places some restrictions on the *SET_NODE_LIST and element geometry, namely that some “tied” elements exist, and the set of “tied” elements consists of exactly two disjoint subsets. The specifics of launching a multi-program MPI program are installation dependent. But the idea behind running a coupled model is that you want to run one set of MPI ranks as if you were running a normal MPP-DYNA job, such as: mpirun –np 4 mppdyna i=input.k memory=200m p=pfile and a second set with just the command line argument “slave” (no input file): mpirun –np 4 mppdyna slave memory=100m p=pfile The main instance knows to look for the slave (because of the presence of the *IN- CLUDE_MULTISCALE_SPOTWELD card), and will run the main model. The “slave” instance will run all the detailed spot weld models. Due to the nature of the coupling, the main model cannot progress when the detailed spot welds are being processed, nor can the detailed spot welds run while the main model is being computed. From a processor efficiency standpoint, it therefore makes sense to run as many slave processes as master processes, and run them on the same CPUs, so that each processing core has one slave and one master process running on it. But you don’t have to – the processes are independent and you can have any number of either. *INCLUDE_TRIM Purpose: This keyword is developed to reduce memory requirements and CPU time (as compared with *INCLUDE) during trimming in sheet metal forming. This keyword is intended to be used together with the *DEFINE_CURVE_TRIM_OPTION and *ELE- MENT_TRIM keywords. Card 1 1 2 3 4 5 6 7 8 Variable Type FILENAME C VARIABLE DESCRIPTION FILENAME File name of the part to be trimmed. General remarks: The name of the file to be trimmed should be included in a usual LS-DYNA input file for trimming, as is in *INCLUDE. Model information, stress and strain tensors should be all in one dynain file generated from LS-DYNA simulation. For example, a drawn panel from a previous simulation can be included in a current trim input file as follows, *INCLUDE_TRIM Drawnpanel.dynain *ELEMENT_TRIM ⋮ *DEFINE_CURVE_TRIM_3D ⋮ *CONTROL_ADAPTIVE_CURVE ⋮ This feature has been developed in conjunction with the Ford Motor Company Research and Advanced Engineering Laboratory, and is implemented in LS-PrePost as of version 4.0 under the metal forming application under eZ-Setup (http://ftp.lstc.com/anonymous/ outgoing/lsprepost/4.0/metalforming/). Compared with *INCLUDE, this keyword draws much less computer memory and runs much faster. Furthermore, in case where to-be-trimmed sheet blank has no stress and strain information (no *INITIAL_STRESS_SHELL, and *INITIAL_STRAIN_SHELL cards present in the sheet blank keyword/dynain file), the bare *INCLUDE keyword must be used. *INCLUDE Referring to the table below (parts courtesy of the Ford Motor Company), compared with simply the keyword *INCLUDE, this keyword reduces memory requirement for trimming by more than 50%. Levels of CPU time reductions vary, in some cases more than 50%. Performance Improvements Roof Hood Inr B-Plr Fender BSA Otr Door Otr Wheel House (2 in 1) Boxside Otr #Element 410810 1021171 351007 189936 380988 315556 261702 1908369 CPU old 7m26s 10m20s 3m11s 2m6s 5m45s 4m27s 2m52s 27m31s new 4m 9m18s 2m56s 1m22s 4m54s 3m35s 2m30s 13m59s Memory (MW) old 282 new 112 616 383 221 117 119 50 233 130 217 114 157 1150 75 539 Revision information: This feature is available in LS-DYNA Revision 62207 or later releases, where the output of strain tensors for the shells is included. Prior Revisions do not include strain tensors for the shells. *INCLUDE_UNITCELL Purpose: This card creates a unit cell model with periodic boundary conditions using *CONSTRAINED_MULTIPLE_GLOBAL. Card 1 1 2 3 4 5 6 7 8 Variable Type Default FILENAME C none Card 2 1 2 3 4 5 6 7 8 Variable INPT OUPT NEDOF Type Default Remarks Card 3 Variable I 0 1 1 DX Type F I 0 2 DY F I 0 2 3 DZ F Default 1.0 1.0 1.0 4 5 6 7 8 NEX NEY NEZ NNPE I 1 I 1 I 1 I Card 4 1 2 3 4 5 6 7 8 Variable NOFF EOFF PNM Type I I I Default none none none Card 5 1 2 3 4 5 6 7 8 Variable CNX CNY CNZ Type I I I Default none none none Node ID Cards. Input is terminated at the next keyword (“*”) card Card 6 1 2 3 4 5 6 7 8 Variable ECNX ECNY ECNZ Type I I I Default none none none VARIABLE DESCRIPTION FILENAME Name of the file containing the information of unit cell. INPT Type of input EQ.0: read *NODE information from the include file and add periodic boundary conditions to the include file. EQ.1: create a unit cell mesh with periodic boundary conditions, and output to the include file. VARIABLE DESCRIPTION OUPT Type of output EQ.1: create a new main keyword file where the keyword *IN- CLUDE_UNITCELL is replaced by *INCLUDE with the include file name. NEDOF Number of extra nodal degrees of freedom (DOFs) for user-defined element. In the current implementation, the limit of NEDOF is 15. DX DY DZ NEX NEY NEZ NNPE Defines the 𝑥-dimension of unit cell. Defines the 𝑦-dimension of unit cell. Defines the 𝑧-dimension of unit cell. Defines number of elements along 𝑥-direction. Defines number of elements along 𝑦-direction. Defines number of elements along 𝑧-direction. Defines number of nodes per element. The current implementation supports only 4-node tetrahedron or 8-node hexahedron elements. NOFF Defines offset of nodal IDs. EOFF PNM CNX CNY CNZ ECNX ECNY Defines offset of elemental IDs. Defines part ID. Defines nodal ID of the 1st control point for the constraint in 𝑥 direction. Defines nodal ID of the 2nd control point for the constraint in 𝑦 direction. Defines nodal ID of the 3rd control point for the constraint in 𝑧 direction. Defines nodal ID of extra control point for the constraint in 𝑥 direction of 3 extra nodal DOFs. Defines nodal ID of extra control point for the constraint in 𝑦 direction of 3 extra nodal DOFs. DESCRIPTION Defines nodal ID of extra control point for the constraint in 𝑧 direction of 3 extra nodal DOFs. VARIABLE ECNZ Remarks: 1. Include File Field. If INPT=0, the geometry and discretization information of unit cell are from the include file. In this case, the parameters in cards 3 and 4 are ignored. 2. Extra Degrees of Freedom. The extra degrees of freedom (DOFs) specified by NEDOF>0 are represented by extra nodes with regular 𝑥, 𝑦 and 𝑧 DOFs. When NEDOF=7, for example, the following chart shows the mapping from the extra DOFs to the regular ones of extra nodes: Extra Node # Extra DOFs Regular DOFs 1 2 3 1 2 3 4 5 6 7 𝑥 𝑦 𝑧 𝑥 𝑦 𝑧 𝑥 In this case, 3 control points for 𝑥, 𝑦, and 𝑧 directions, respectively, need to be defined for each extra node. The keyword *INITIAL provides a way of initializing velocities and detonation points. The keyword control cards in this section are defined in alphabetical order: *INITIAL_AIRBAG_PARTICLE_POSITION *INITIAL_ALE_MAPPING *INITIAL_AXIAL_FORCE_BEAM *INITIAL_CONTACT_WEAR *INITIAL_DETONATION *INITIAL_EOS_ALE *INITIAL_FATIGUE_DAMAGE_RATIO *INITIAL_FIELD_SOLID *INITIAL_FOAM_REFERENCE_GEOMETRY *INITIAL_GAS_MIXTURE *INITIAL_HYDROSTATIC_ALE *INITIAL_IMPULSE_MINE *INITIAL_INTERNAL_DOF_SOLID_{OPTION} *INITIAL_LAG_MAPPING *INITIAL_MOMENTUM *INITIAL_PWP_DEPTH *INITIAL_STRAIN_SHELL_{OPTION} *INITIAL_STRAIN_SOLID_{OPTION} *INITIAL_STRAIN_TSHELL *INITIAL_STRESS_BEAM *INITIAL_STRESS_DEPTH *INITIAL_STRESS_SECTION *INITIAL_STRESS_SOLID *INITIAL_STRESS_SPH *INITIAL_STRESS_TSHELL *INITIAL_TEMPERATURE_{OPTION} *INITIAL_VEHICLE_KINEMATICS There are two alternative sets of keywords for setting initial velocities. Cards from one set cannot be combined with cards from the other. Standard velocity cards: *INITIAL_VELOCITY *INITIAL_VELOCITY_NODE *INITIAL_VELOCITY_RIGID_BODY Alternative initial velocity cards supporting initial rotational about arbitrary axes and start times. Alternative velocity cards: *INITIAL_VELOCITY_GENERATION *INITIAL_VELOCITY_GENERATION_START_TIME *INITIAL_VOID_{OPTION} *INITIAL_VOLUME_FRACTION *INITIAL_VOLUME_FRACTION_GEOMETRY *INITIAL_AIRBAG_PARTICLE_POSITION Purpose: This card initializes the position of CPM initial air particle to the location specified. Card 1 1 2 3 4 5 6 7 8 Variable Bag_ID Type I Default none Particle Cards. The ith card specifies the location of the ith particle. LS-DYNA expects one card for each particle, if fewer cards are supplied the coordinates will be reused and particles may share the same location at the beginning of the simulation. 5 6 7 8 Card 1 Variable Type 8x Default 2 X F 3 Y F 4 Z F VARIABLE DESCRIPTION Bag_ID Airbag ID defined in *AIRBAG_PARTICLE_ID card X Y Z 𝑥 coordinate 𝑦 coordinate 𝑧 coordinate *INITIAL_ALE_MAPPING Purpose: This card initializes the current ALE run with data from the last cycle of a previous ALE run. Data are read from a mapping file specified by “map=” on the command line . To map data histories (not just the last cycle) to a region of selected elements see *BOUNDARY_ALE_MAPPING. The following transitions are allowed: 1D → 2D 1D → 3D 2D → 2D 2D → 3D 3D → 3D 3D → 2D Card 1 1 2 3 4 5 6 7 8 Variable PID TYP AMMSID Type I I I Default none none none Card 2 Variable 1 XO Type F 2 YO F 3 ZO F 4 5 6 7 8 VECID ANGLE I F Default 0.0 0.0 0.0 none none VARIABLE DESCRIPTION PID TYP Part ID or part set ID. Type of “PID” : EQ.0: part set ID (PSID). EQ.1: part ID (PID). AMMSID Set ID of ALE multi-material groups defined in *SET_MULTI- MATERIAL_GROUP. See Remark 1. XO Origin position in global 𝑥-direction. See Remarks 2 and 5. VARIABLE DESCRIPTION Origin position in global 𝑦-direction. See Remarks 2 and 5. Origin position in global 𝑧-direction. See Remarks 2 and 5. ID of the symmetric axis defined by *DEFINE_VECTOR. See Remarks 3 and 5. Angle of rotation in degrees around an axis defined by *DE- FINE_VECTOR for the 3D to 3D mapping. See Remark 4. YO ZO VECID ANGLE Remarks: 1. Mapping of Ale Multi-Material Groups. The routines of this card need to know which mesh will be initialized with the mapping data, and more specifi- cally, which multi-material groups. The first two fields, PID, and TYP, define the mesh. The third field, AMMSID, refers to a multi-material group list ID; see the *SET_MULTI-MATERIAL_GROUP_LIST card. The group list AMMSID should have as many elements as there are groups in the previous calculation . Example: If the previous model has 3 groups, the current one has 5 groups and the following mapping is wanted. Group 1 from the previous run → Group 3 in the current run Group 2 from the previous run → Group 5 in the current run Group 3 from the previous run → Group 4 in the current run The *SET_MULTI-MATERIAL_GROUP_LIST card should be set as follows: *SET_MULTI-MATERIAL_GROUP_LIST 300 3,5,4 In special cases, a group can be replaced by another. If the group 4 in the pre- vious example should be replaced by the group 3, the keyword setup would be modified to have -3 instead of 4. The minus sign is a way for the code to know that the replacing group (-3 replaces 4) is a complement of the group 3: *SET_MULTI-MATERIAL_GROUP_LIST 300 3,5,-3 2. Coordinate System Origin. The location to which the data is mapped is controlled by the origin of the coordinate system (XO, YO, ZO). 3. Symmetry Axis. For a mapping file created by a previous asymmetric model, the symmetric axis orientation in the current model is specified by VECID. For a mapping file created by a 3D or 1D spherical model, the vector VECID is read but ignored. For a 3D to 3D mapping the vector is used if the parameter AN- GLE is defined . 4. Rotating 3D Data Onto a 3D calculation. For a mapping from a previous 3D run to a current 3D model the previous 3D data will be rotated about the vector, VECID, through an angle specified in the ANGLE field. 5. Plain Strain, and 3D to 2D. The definitions of X0, Y0, Z0 and VECID change in the case of the following mappings: a) plain strain 2D (ELFORM = 13 in *SECTION_ALE2D) to plain strain 2D b) plain strain 2D to 3D c) 3D to 2D While, VECID still defines the y-axis in the 2D domain, the 3 first parameters in *DEFINE_VECTOR, additionally, define the location of the origin. The 3 last parameters defines a position along the y-axis. For this case when 2D data is used in a 3D calculation the point X0, Y0, Z0 together with the vector, VECID, define the plane. 6. Mapping File. Including the command line argument “map=” will invoke the creation of a mapping file. When the keyword INITIAL_ALE_MAPPING is not in the input deck, but the argument “map=” is present on the command line, the ALE data from the last cycle is written in the mapping file. This file con- tains the following nodal and element data: • nodal coordinates (last step) • nodal velocities • part ids • element connectivities • element centers • densities • volume fractions • stresses • plastic strains • internal energies • bulk viscosities *INITIAL Chained Mappings. To chain mapping operations so that LS-DYNA both reads and writes a mapping file the command line argument “map1=” is neces- sary. If the keyword INITIAL_ALE_MAPPING is in the input deck and the prompt “map=” is in the command line, the ALE data is read from the mapping file defined by “map=” to initialize the run. Data from the last cycle are written in the mapping file defined by “map1=”. *INITIAL_AXIAL_FORCE_BEAM Purpose: Initialize the axial force resultants in beam elements that are used to model bolts. This option works with *MAT_SPOTWELD with beam type 9, a Hughes-Liu type beam. Card 1 1 2 3 4 5 6 7 8 Variable BSID LCID SCALE KBEND Type I I F Default none none 1.0 I 0 VARIABLE DESCRIPTION BSID LCID Beam set ID. Load curve ID defining preload force versus time. When the load curve ends or goes to zero, the initialization is assumed to be completed. See Remark 2 below. SCALE Scale factor on load curve. KBEND Bending stiffness flag EQ.0: Bending stiffness is negligible since all integration points are assigned the same axial stress EQ.1: Bending stiffness is retained by keeping the axial stress gradient Remarks: 1. Damping. To achieve convergence during explicit dynamic relaxation, the application of the damping options is very important. If contact is active, con- tact damping is recommended with a value between 10-20 percent. Additional damping, via the option DAMPING_PART_STIFFNESS also speeds conver- gence where a coefficient of 0.10 is effective. If damping is not used, conver- gence may not be possible. 2. Ramping. When defining the load curve, LCID, a ramp starting at the origin should be used to increase the force to the desired value. The time duration of the ramp should produce a quasistatic response. When the end of the load curve is reached, or when the value of the load decreases from its maximum value, the initialization stops. If the load curve begins at the desired force val- ue, i.e., no ramp, convergence will take much longer, since the impulsive like load created by the initial force can excite nearly every frequency in the struc- tural system where force is initialized. *INITIAL_CONTACT_WEAR Purpose: Initialize contact wear for simulation of wear processes, define as many cards as necessary. Card 1 1 2 3 4 Variable CID NID WDEPTH NX Type I I F F 5 NY F 6 NZ F 7 8 ISEQ NCYC I I Default none none none none none none none none VARIABLE DESCRIPTION CID NID Contact Interface ID. Node ID. WDEPTH Wear depth, in units of length. NX, NY, NZ Direction vector for wear, internally normalized. Simulation sequence number for the entire process. The wear on this card will be processed NCYC times to modify the worn geometry. This is to say that one LS-DYNA simulation is used to predict the wear for NCYC repetitions of the process, in order to save simulation time. This number should be chosen with care, a negative number means that LS-DYNA will not apply this card, see remarks below. ISEQ NCYC Remarks: This is a card that is not supposed to be manually inserted, but is automatically generated by LS-DYNA when simulating wear processes, see *CONTACT_ADD_- WEAR and parameters NCYC on *INTERFACE_SPRINGBACK_LSDYNA and SPR/MPR on *CONTACT. A sequence of identical simulations, except for perturbation of the geometry of certain components due to wear, is undertaken. For a given contact interface and node ID, the corresponding node is perturbed by the wear depth in the direction of wear. If the cycle number NCYC is negative, this means that the geometry has been already processed in LS-PrePost and the card is ignored by LS-DYNA, and if a node appears multiple times the wear from the individual sequences is accumulated. *INITIAL_CRASHFRONT Purpose: To define initial crashfront node set for materials supporting crashfront. Card 1 1 2 3 4 5 6 7 8 Variable SID STYPE Type I Default none I 0 VARIABLE DESCRIPTION SID Crash front node set ID for initial crashfront nodes. STYPE ID type of SID: EQ.0: segment set ID, EQ.1: shell element set ID, EQ.2: part set ID, EQ.3: part ID, EQ.4: node set ID. Remarks: Material models 17, 54, 55, 58, 169, 261, and 262 reduce material strength in crashfront elements. This keyword defines the initial crashfront nodes, and all elements connected to these nodes are initialized as crashfront elements with reduced strength. *INITIAL Purpose: Define points to initiate the location of high explosive detonations in part ID’s which use *MAT_HIGH_EXPLOSIVE_BURN (*MAT_008). Also see *CONTROL_EX- PLOSIVE_SHADOW. If no *INITIAL_DETONATION is defined, detonation occurs in all the high explosive elements at time = 0. 6 7 8 Card 1 1 Variable PID Type I 2 X F 3 Y F 4 Z F Default all HE 0. 0. 0. 5 LT F 0. Accoustic Boundary Card. Additional card for PID = -1. Card 2 1 2 Variable PEAK DECAY Type Remark F 1 F 1 3 XS F 4 YS F 5 ZS F 6 NID I 7 8 VARIABLE PID DESCRIPTION Part ID of the high explosive to be lit, except in the case where the high explosive is modeled using an ALE formulation, in which case PID is the part ID of the mesh where the high explosive material to be lit initially resides. However, two other options are available: EQ.-1: an acoustic boundary, also, *BOUNDARY_USA_SUR- FACE, EQ.0: all high explosive materials are considered. X Y 𝑥-coordinate of detonation point, see Figure 23-1. 𝑦-coordinate of detonation point. Z LT *INITIAL_DETONATION DESCRIPTION 𝑧-coordinate of detonation point. Lighting time for detonation point. This time is ignored for an acoustic boundary. PEAK Peak pressure, po, of incident pressure pulse, see remark below. DECAY Decay constant, τ XS YS ZS 𝑥-coordinate of standoff point, see Figure 23-1. 𝑦-coordinate of standoff point 𝑧-coordinate of standoff point NID Reference node ID near structure Pressure profile at standoff point Standoff point Structure Reference node where pressure begins at t=0. This node is typically one element away from the structure. Acoustic mesh boundary is treated as a transmitting boundary. Detonation point Figure 23-1. Initialization of the initial pressures due to an explosive disturbance is performed in the acoustic media. LS-DYNA automatically determines the acoustic mesh boundary and applies the pressure time history to the boundary. This option is only applicable to the acoustic element formulation, see *SECTION_SOLID. Remarks: For solid elements (not acoustic) two options are available. If the control card option, *CONTROL_EXPLOSIVE_SHADOW, is not used the lighting time for an explosive element is computed using the distance from the center of the element to the nearest detonation point, 𝐿𝑑; the detonation velocity, 𝐷; and the lighting time for the detonator, 𝑡𝑑: 𝑡𝐿 = 𝑡𝑑 + 𝐿𝑑 . The detonation velocity for this default option is taken from the element whose lighting time is computed and does not account for the possibilities that the detonation wave may travel through other explosives with different detonation velocities or that the line of sight may pass outside of the explosive material. If the control card option, *CONTROL_EXPLOSIVE_SHADOW, is defined, the lighting time is based on the shortest distance through the explosive material. If inert obstacles exist within the explosive material, the lighting time will account for the extra time required for the detonation wave to travel around the obstacles. The lighting times also automatically accounts for variations in the detonation velocity if different explosives are used. No additional input is required for this option but care must be taken when setting up the input. This option works for two and three-dimensional solid elements. It is recommended that for best results: 1. Keep the explosive mesh as uniform as possible with elements of roughly the same dimensions. 2. Inert obstacle such as wave shapers within the explosive must be somewhat larger than the characteristic element dimension for the automatic tracking to function properly. Generally, a factor of two should suffice. The characteristic element dimension is found by checking all explosive elements for the largest diagonal. 3. The detonation points should be either within or on the boundary of the explosive. Offset points may fail to initiate the explosive. When LT is nonzero, the detonation point is fixed to the explosive material at t = 0 and moves as the explosive material moves prior to detonation. 4. Check the computed lighting times in the post processor LS-PREPOST. The lighting times may be displayed at time = 0., state 1, by plotting component 7 (a component normally reserved for plastic strain) for the explosive material. The lighting times are stored as negative numbers. The negative lighting time is replaced by the burn fraction when the element ignites. Line detonations may be approximated by using a sufficient number of detonation points to define the line. Too many detonation points may result in significant initialization cost. The pressure versus time curve for the acoustic option is defined by: 𝑝(𝑡) = 𝑝𝑜𝑒− 𝑡 𝜏. *INITIAL Purpose: This card initializes the pressure in ALE elements that have materials with *EOS. Card 1 Variable 1 ID 2 3 TYP MMG Type I I I 4 E0 F 5 V0 F 6 P0 F 7 8 Default none none none 0.0 0.0 0.0 VARIABLE DESCRIPTION ID TYP Part ID or part set ID or element set ID. Type of “ID”: EQ.0: part set ID. EQ.1: part ID. EQ.2: element set ID (*SET_BEAM in 1D, *SET_SHELL in 2D, *SET_SOLID in 3D). MMG Specifies the multi-material group. GT.0: ALE multi-material group. LT.0: Set ID of ALE multi-material groups defined in *SET_- MULTI-MATERIAL_GROUP. Initial internal energy per reference volume unit (as defined in *EOS). See Remark 1. Initial relative volume (as defined in *EOS). See Remark 1. Initial pressure. See Remark 2. E0 V0 P0 Remarks: 1. Initialization with Volume and Energy. For most *EOS, E0 and V0 should be used to initialize the pressure. If only the internal energy is initialized, V0 should be 1.0 ( If V0 = 0.0, E0 will not be applied). 2. Initial Pressure with Derived Volume and Energy. For *EOS_001, *EOS_004 and *EOS_006, the initial pressure P0 can be input directly. An iterative meth- od will compute the initial internal energy and relative volume. This approach is applied if E0 = 0.0 and V0 = 0.0. *INITIAL_FATIGUE_DAMAGE_RATIO_{OPTION} Available options include: <BLANK> BINARY Purpose: This card sets initial damage ratio for fatigue analysis. The initial damage ratio may come from the previous loading cases. The initial damage ratio can be defined by user directly, or can be extracted from existing binary database like D3FTG (using the option BINARY). Card 1 for no option, <BLANK>. Card 1 1 2 3 4 5 6 7 8 Variable PID/SID PTYP DRATIO Type I Default none I 0 F 0.0 Card 1 for option BINARY. Card 1 1 2 3 4 5 6 7 8 Variable Type Default FILENAME C d3ftg VARIABLE DESCRIPTION PID/SID Part ID or part set ID for which the initial damage ratio is defined. PTYP Type of PID/SID: EQ.0: part ID. EQ.1: part set ID. *INITIAL_FATIGUE_DAMAGE_RATIO DESCRIPTION DRATIO Initial damage ratio. FILENAME Path and name of existing binary database information. for fatigue Remarks: 1. The card works for both time domain fatigue and frequency domain fatigue problems. 2. Card 1 can be repeated if the model has initial damage ratio coming from multiple loading cases. *INITIAL Purpose: This keyword is a simplified version of *INITIAL_STRESS_SOLID which can be used with hyperelastic materials. The keyword is used for history variable input. Data is usually in the form of the eigenvalues of diffusion tensor data. These are expressed in the global coordinate system. The input deck takes the following parameters: NOTE: As of LS-DYNA R5 in all contexts, other than *MAT_TISSUE_DISPERSED, this keyword is depre- cated (and disabled). For all other materials this keyword has been superceded by *INITIAL_- STRESS_SOLID. Include as many pairs of cards 1 and 2 as necessary. This input ends at the next keyword (“*”) card. Card 1 1 2 3 4 5 6 7 8 Variable EID NINT NHISV Type I I Default none none Card 2 1 2 I 0 3 4 5 6 7 8 Variable FLD1 FLD2 FLD3 FLD4 FLD5 FLD6 FLD7 FLD8 Type F F F F F F F F Default VARIABLE DESCRIPTION EID NINT Element ID Number of integration points (should correspond to the solid element formulation). NHISV *INITIAL_FIELD_SOLID DESCRIPTION Number of field variables. If NHISV exceeds the number of integration point field variables required by the constitutive model, only the number required is output; therefore, if in doubt, set NHISV to a large number. FLDn Data for the nth field (history) variable. NOTE that *MAT_TIS- SUE_DISPERSED only use FLD1 to FLD3 since NHISV = 3. Remarks: Add as many cards as necessary. The keyword input ends when next keyword appears (next *). For example for two elements it can look as: *INITIAL_FIELD_SOLID $EID NINT NHISV 1 1 3 $FLD1 FLD2 FLD3 0.1 0.8 0.1 $EID NINT NHISV 2 1 3 $FLD1 FLD2 FLD3 0.3 0.2 0.5 *INITIAL_FOAM_REFERENCE_GEOMETRY_OPTION Available options include: RAMP Purpose: The reference configuration allows stresses to be initialized (via REF in *MAT) in the following hyperelastic material models: 2, 5, 7, 21, 23, 27, 31, 38, 57, 73, 77, 83, 132, 179, 181, 183, and 189. Supported solid elements are the constant stress hexahedron (#1), the fully integrated S/R hexahedron (#2), the tetrahedron (#10), and the pentahedron (#15). To use this option, the geometry of the foam material is defined in a deformed configuration. The stresses in the low density foam then depend only on the deformation gradient matrix 𝐹𝑖𝑗: 𝐹𝑖𝑗 = ∂𝑥𝑖 ∂𝑋𝑗 where 𝑥𝑖 is the deformed configuration and 𝑋𝑗 is the undeformed configuration. By using this option, dynamic relaxation can be avoided once a deformed configuration is obtained usually on the first run of a particular problem. Optional RAMP Card. Additional optional card for the option of RAMP. Card 1 1 2 3 4 5 6 7 8 Variable NDTRRG Type Default I Include as many cards as necessary. This input ends at the next keyword (“*”) card. Card 1 1 2 3 4 5 6 7 8 9 10 Variable NID Type I X F Default none 0. Y F 0. Z F 0. Remarks VARIABLE NDTRRG DESCRIPTION Number of time steps taken for an element to restore its reference geometry. Definition of NDTRRG allows an element to ramp up to its reference shape in NDTRRG time steps. Currently ls-dyna uses only one NDTRRG and applies it to all foam materials with reference geometries. If more than one NDTRRG is defined, the latter defined one will replace the previously define one. NID Node number X Y Z 𝑥 coordinate in reference configuration 𝑦 coordinate in reference configuration 𝑧 coordinate in reference configuration *INITIAL Purpose: This command is used to specify (a) which ALE multi-material groups may be present inside an ALE mesh set at time zero, and (b) the corresponding reference gas temperature and density which define the initial thermodynamic state of the gases. The order of the species in the gas mixture corresponds to the order of different gas species defined in the associated *MAT_GAS_MIXTURE card. This card must be used together with a *MAT_GAS_MIXTURE (or equivalently, a *MAT_ALE_GAS_MIXTURE) card. Card 1 1 2 3 4 5 6 7 8 Variable SID STYPE MMGID TEMP Type I Default none Card 2 1 I 0 2 I F none none 3 4 5 6 7 8 Variable RO1 RO2 RO3 RO4 RO5 RO6 RO7 RO8 Type F F F F F F F F Default 0.0 0.0 0.0 0.0 0.0 0.0 0.0 0.0 VARIABLE SID DESCRIPTION Set ID for initialization. This SID defines the ALE mesh within which certain ALE multi-material group(s) may be present at 𝑡 = 0. STYPE Set type for the SID above: EQ.0: SID is a part set ID EQ.1: SID is a part ID MMGID ALE Multi-material group ID of the material that may be present at t = 0 in the ALE mesh set defined by SID. Initial static temperature of the gas species occupying the ALE mesh. Note that all species in the mixture are assumed to be in thermal equilibrium (having the same 𝑇). Initial densities of the ALE material(s) which may be occupying some region (or all) of the aforementioned ALE mesh, for up to eight different gas species. The order of the density input corresponds to the order of the materials defined in associated *MAT_GAS_MIXTURE card. *INITIAL VARIABLE TEMP RO1-RO8 Remarks: 1. Please see the example under the *MAT_GAS_MIXTURE card definition for an application of the *INITIAL_GAS_MIXTURE card. 2. The temperature is assumed to be the initial temperature which together with the gas density, will define the initial pressure of the gas species via the perfect gas law, The user should manually check the initial pressure for consistency. 𝑃|𝑡=0 = 𝜌∣𝑡=0(𝐶𝑃 − 𝐶𝑉)𝑇|𝑡=0. 3. Given an ALE mesh, this mesh may initially be occupied by one or more ALE multi-material groups (AMMG). For example, a background ALE mesh (H1) containing AMMG 1 may be partially filled with AMMG 2 via the volume fill- ing command *INITIAL_VOLUME_FRACTION_GEOMETRY. Then there are 2 AMMGs to be initialized for this mesh H1. The commands look like the follow- ing. $--------------------------------------------------------------------------- $ One card is defined for each AMMG that will occupy some elements of a mesh set *INITIAL_GAS_MIXTURE $ SID STYPE MMGID T0 1 1 1 298.15 $ RHO1 RHO2 RHO3 RHO4 RHO5 RHO6 RHO7 RHO8 1.0E-9 *INITIAL_GAS_MIXTURE $ SID STYPE MMGID T0 1 1 2 298.15 $ RHO1 RHO2 RHO3 RHO4 RHO5 RHO6 RHO7 RHO8 1.2E-9 $--------------------------------------------------------------------------- *INITIAL Purpose: When an ALE model contains one or more regular (not reservoir-type) ALE parts (ELFORM = 11 and AET = 0), this command may be used to initialize the hydrostatic pressure field in the regular ALE domain due to gravity. The *LOAD_- BODY_(OPTION) keyword must be defined. Card 1 1 2 3 4 5 6 7 8 Variable ALESID STYPE VECID GRAV PBASE Type I Default none I 0 I none I 0 I 0 Multi-material Layers Group Cards. Repeat card 2 as many times as the number of AMMG layers present in the model. Card 2 1 2 3 4 5 6 7 8 Variable NID MMGBLO Type I I Default none none VARIABLE ALESID DESCRIPTION ALESID is a set ID defining the ALE domain/mesh whose hydrostatic pressure field due to gravity is being initialized by this keyword. See Remark 2 and 4. STYPE ALESID set type. See Remark 4. EQ.0: Part set ID (PSID), EQ.1: Part ID (PID), EQ.2: Solid set ID (SSID). VECID Vector ID of a vector defining the direction of gravity. GRAV PBASE *INITIAL_HYDROSTATIC_ALE DESCRIPTION Magnitude of the Gravitational acceleration. For example, in metric units the value is usually set to 9.80665 m/s2. Nominal or reference pressure at the top surface of all fluid layers. By convention, the gravity direction points from the top layer to the bottom layer. Each fluid layer must be represented by an ALE multi-material group ID (AMMGID or MMG). See Remark 1. NID Node ID defining the top of an ALE fluid (AMMG) layer. MMGBLO AMMG ID of the fluid layer immediately below this NID. Each node is defined in association with one AMMG layer below it. See Remark 3. Remarks: 1. Pressure in Multi-Layer Fluids. For models using multi-layer ALE Fluids the pressure at the top surface of the top fluid layer is set to PBASE and the hydro- static pressure is computed as following 𝑁layers 𝑃 = 𝑃base + ∑ 𝜌𝑖𝑔ℎ𝑖 . 𝑖=1 2. Limitations on Element Formulation. The keyword applies only to the regular ALE parts with ELFORM = 11 and AET = 0 on the *SECTION_SOLID and *SECTION_ALE2D cards (not reservoir-type). This keyword cannot be used to initialize reservoir-type ALE parts (AET = 4). Also, ramping functions are not supported, so the loading is done in one step at 𝑡 = 0. For initializing reservoir-type ALE domain, please review the *ALE_AMBIENT_HYDROSTAT- IC keyword. 3. Limitation on EOS Model. The keyword only supports *EOS_GRUNEISEN and *EOS_LINEAR_POLYNOMIAL, but only inthe following two cases, 𝑐4 = 𝑐5 > 0, 𝑐3 = 𝑐4 = 𝑐5 = 𝑐6 = 0, 𝑐1 = 𝑐2 = 𝑐3 = 𝑐6 = 0, 𝐸0 = 0 𝑉0 = 0. 4. Structured ALE usage. When used with structured ALE, PART and PART set options might not make too much sense. This is because all elements inside a structured ALE mesh are assigned to one single PART ID. If we want to pre- scribe initial hydrostatic pressure for all the elements inside the structured mesh, we can certainly use that PART ID. But if we only want to do that to some elements, we have to generate a solid set which contains those structured ALE elements. It is done by using the *SET_SOLID_GENERAL keyword with SALECPT option. And then use STTYPE=2 (solid element set ID) option. Example: Model Summary: Consider a model consisting of 2 ALE parts, air on top of water. H1 = AMMG1 = Air part above. H2 = AMMG2 = Water part below. $...|....1....|....2....|....3....|....4....|....5....|....6....|....7....|....8 $ (non-ambient) ALE materials (fluids) listed from top to bottom: $ $ NID AT TOP OF A LAYER SURFACE ALE MATERIAL LAYER BELOW THIS NODE $ TOP OF 1st LAYER -------> 1722 ---------------------------------------- $ Air above = PID 1 = H1 = AMMG1 (AET=0) $ TOP OF 2nd LAYER -------> 1712 ---------------------------------------- $ Water below = PID 2 = H2 = AMMG2 (AET=0) $ BOTTOM ----------------------------------------------------------------------- $...|....1....|....2....|....3....|....4....|....5....|....6....|....7....|....8 *INITIAL_HYDROSTATIC_ALE $ ALESID STYPE VECID GRAV PBASE 12 0 11 9.80665 101325.0 $ NID MMGBLO 1722 1 1712 2 *SET_PART_LIST 12 1 2 *ALE_MULTI-MATERIAL_GROUP 1 1 2 1 *DEFINE_VECTOR $ VID XT YT ZT XH YH ZH CID 11 0.0 1.0 0.0 0.0 0.0 0.0 *DEFINE_CURVE 9 0.000 0.000 0.001 1.000 10.000 1.000 *LOAD_BODY_Y $ LCID SF LCIDDR XC YC ZC 9 9.80665 0 0.0 0.0 0.0 $...|....1....|....2....|....3....|....4....|....5....|....6....|....7....|....8 *INITIAL_IMPULSE_MINE Purpose: Apply initial velocities to the nodes of a 3D structure due to the impulse imparted by the detonation of a buried land mine. This feature is based on the empirical model developed by [Tremblay 1998]. Card 1 1 Variable SSID Type I 2 M F 3 4 5 6 7 8 RHOS DEPTH AREA SCALE not used UNIT F F F F Default none 0.0 0.0 0.0 0.0 1.0 I 1 Remarks 1 2 Either set a heading or delete this row. Card 1 Variable Type 1 X F 2 Y F 3 Z F Default 0.0 0.0 0.0 4 5 6 7 8 NIDMC GVID TBIRTH PSID SEARCH I 0 I F none 0.0 I 0 F 0.0 VARIABLE DESCRIPTION SSID Segment set ID MTNT RHOS DEPTH Equivalent mass of TNT . Density of overburden soil. Burial depth from the ground surface to the center of the mine. This value must be a positive. AREA Cross sectional area of the mine. SCALE Scale factor for the impulse. VARIABLE UNIT DESCRIPTION Unit system. This must match the units used by finite element model. EQ.1: inch, dozen slugs (i.e., lbf × s2/in), second, PSI (default) EQ.2: meter, kilogram, second, Pascal EQ.3: centimeter, gram, microsecond, megabar EQ.4: millimeter, kilogram, millisecond, GPa EQ.5: millimeter, metric ton, second, MPa EQ.6: millimeter, gram, millisecond, MPa X, Y, Z 𝑥-, 𝑦-, and 𝑧- coordinates of mine center. NIDMC GVID Optional node ID representing the mine center . If defined then X, Y and Z are ignored. Vector ID representing the vertically upward direction, i.e., normal to the ground surface . TBIRTH Birth time. Impulse is activated at this time. Part set ID identifying the parts affected by the mine . If zero it defaults to the part comprised by the nodes of the segment set. Limit the search depth into the structure. Initial nodal velocity is distributed from the segment to a depth equal to the SEARCH value. The value must be positive. If set to zero the search depth is unlimited and extends through the part(s) identified by PSID. PSID SEARCH Remarks: 1. Segment normals should nominally point toward the mine. 2. The segments should belong to 3D thin shell, solid, or thick shell elements. This feature cannot be applied to 2D geometries. 3. Several methods can be used to approximate the equivalent mass of TNT for a given explosive. One method involves scaling the mass by the ratio of the squares of the Chapman-Jouguet detonation velocities given by the relation- ship. z GVID mine soil (𝑥, 𝑦, 𝑧) Figure 23-2. Schematic of the buried mine parameters. 𝑀TNT = 𝑀 (DCJ)2 (DCJ)TNT is the Chapman-Jouguet where 𝑀TNT is the equivalent TNT mass and (DCJ)TNT detonation velocity of TNT. 𝑀 and DCJ are, respectively, the mass and C-J velocity of the explosive under investigation. “Standard” TNT is considered to be cast with a density of 1.57gm/cm3 and (DCJ)TNT = 0.693 cm/𝜇sec. 4. This implementation assumes the energy release (heat of detonation) for 1 kilogram of TNT is 4.516 MJ. 5. Prediction of the impulse relies on an empirical approach which involves fitting curves to experimental results. The upper error bound is 1.8 times the predict- ed value and the lower is predicted value divided by 1.8. Thus, if the predicted impulse is 10 kN-seconds then the solution space ranges from 5.6 kN-sec to 18 kN-sec. 6. The computed impulse is valid when the following criteria are met. 0.106 ≤ 6.35 ≤ 𝐸 𝐴⁄ 𝜌𝑐2𝑧 ≤ 1 ≤ 150 0.154 ≤ 0 ≤ √𝐴 ≤ 4.48 ≤ 19.3 where, 𝛿 = the distance from the mine center to the ground surface (DEPTH) 𝑧 = the vertical distance from the mine center to the target point 𝐸 = the energy release of the explosive 𝐴 = the cross-sectional area of the mine (AREA) 𝜌 = the soil density (RHOS) 𝑐 = the wave speed in the soil 𝑑 = the lateral distance from the mine center to the target point. See Figure 23-2. References: Tremblay, J.E., “Impulse on Blast Deflectors from a Landmine Explosion,” DRDC Valcartier, DREV-TM-9814, (1998). *INITIAL_INTERNAL_DOF_SOLID_OPTION Available Options Include: TYPE3 TYPE4 Purpose: Initialize the internal degrees of freedom for solid element types 3 and 4. Card 1 1 2 3 4 5 6 7 8 Variable LID Type I Default none Value Cards. Include 12 cards TYPE3 and 6 cards for TYPE4. Card 1 2 3 4 5 6 7 8 Variable VALX VALY VALZ Type F F F Default none none none VARIABLE DESCRIPTION LID VALX VALY VALZ Element ID. 𝑥 component of internal degree of freedom. 𝑦 component of internal degree of freedom. 𝑧 component of internal degree of freedom. Remarks: 1. The internal degrees of freedom are specified in terms of the displacements of the corresponding mid-side nodes of the 20 node hex and the 10 node tetrahe- dron that are the basis of the type 3 and 4 solid elements, respectively. The available options are <BLANK> WRITE *INITIAL_LAG_MAPPING Purpose: This card initializes a 3D Lagrangian calculation with data from the last cycle of a preceding 2D or 3D Lagrangian calculation. In its *INITIAL_LAG_MAPPING form (<BLANK> option), this keyword causes data to be read in from a mapping file; while, with the WRITE active this card is used to set which parts are written to the mapping file. The mapping file’s filename is specified using the “lagmap=” command line argument . Card 1 1 2 3 4 5 6 7 8 Variable SETID Type I Default none Card 2. Additional card for <BLANK> keyword option. 4 5 6 7 8 VECID ANGLE NELANGL Card 2 Variable 1 XP Type F 2 YP F 3 ZP F I F I 0 Default 0.0 0.0 0.0 none none VARIABLE DESCRIPTION SETID part set ID. See Remarks 3 and 4. XP 𝑥-position of a point belonging to the plane from which the 3D mesh is generated (only for a 2D to 3D mapping). See Remark 5. VARIABLE DESCRIPTION YP ZP VECID ANGLE 𝑦-position of a point belonging to the plane from which the 3D mesh is generated (only for a 2D to 3D mapping). See Remark 5. 𝑧-position of a point belonging to the plane from which the 3D mesh is generated (only for a 2D to 3D mapping). See Remark 5. ID of the rotation axis (symmetric axis for a 2D to 3D mapping) defined by *DEFINE_VECTOR. See Remark 5. Angle of rotation around an axis defined by *DEFINE_VECTOR. See Remark 5. NELANGL Number of elements to create in the azimuthal direction for ANGLE (only for a 2D to 3D mapping). See Remark 5. Remarks: part ids nodal velocities nodal coordinates (initial and last steps) nodal temperatures (if *CONTROL_THERMAL_SOLVER is used) 1. The Mapping File as Output. In the absence of a *INITIAL_LAG_MAPPING card, adding a “lagmap=” argument to the command line will cause LS-DYNA to write a mapping file. This file contains the following nodal and element data: • • • • • • • • • • • • • element connectivities volume fractions internal energies relative volumes element centers bulk viscosities plastic strains densities stresses 2. The Mapping File as Input. If the keyword INITIAL_LAG_MAPPING is in the input deck and the “lagmap=” argument is in the command line, then La- grangian data is read from the mapping file defined by “lagmap=” to initialize the run. 3. Part Sets (Write). The part set, SETID, defines which parts are involved in the mapping. The WRITE option can be used to write data in the mapping file for ONLY the parts specified by the set. If the keyword INITIAL_LAG_MAP- PING_WRITE is not included in the input deck then ALL Lagrangian parts are written in the mapping file during the last cycle. Similarly, for reading 4. Part Sets (Read). The mapping initializes the data for every node and element defined by SETID within the domain swept by the 2D mesh or the region ini- tially occupied by the previous 3D mesh. For nodes and elements outside of SETID it has no effect. 5. Embedding. The first point in the definition of the rotation axis VECID specifies the origin location for the previous run in the current 3D space. The 2D to 3D mapping depends on whether or not a 3D mesh has already been defined. The 3D to 3D mapping needs a pre-existing mesh. a) No Mesh Case for a 2D to 3D mapping. If there is no 3D mesh (no solid and shell with parts in SETID), the point (XP, YP, ZP) together with the sym- metry axis (VECID) are used to generate a mesh. The point defines the plane in which the 2D is embedded. The 3D mesh is generated by rotating the 2D mesh around the axis. The point (XP, YP, ZP) must not be on the symmetry axis. ANGLE defines the angle of rotation in degrees. The ro- tation is counterclockwise when viewed from the axis head. NELANGL is the number of elements to generate in the azimuthal direction. b) Pre-existing Mesh Case for a 2D to 3D mapping. If there is a 3D mesh (solids or shells with parts in SETID), the nodes should be within the domain swept by the initial positions of the 2D mesh. Then, the nodes are mapped to new locations based on the last mesh positions of the previous run. c) Pre-existing Mesh Case for a 3D to 3D mapping. If there is a 3D mesh (solids or shells with parts in SETID), the nodes should be in the region initially occupied by the previous 3D mesh. Then, the nodes are mapped to new locations based on the last mesh positions of the previous run. VECID is an axis of rotation of the pre-existing mesh if ANGLE is defined. If this latter is not defined, the first point in VECID is still the previous origin lo- cation and it can be used to translate the pre-existing mesh *INITIAL Purpose: Define initial momentum to be deposited in solid elements. This option is to crudely simulate an impulsive type of loading. Card 1 Variable EID 2 MX Type I F Default none 0. 3 MY F 0. 4 5 6 7 8 MZ DEPT F 0. F 0, VARIABLE DESCRIPTION EID MX MY MZ Element ID Initial 𝑥-momentum Initial 𝑦-momentum Initial 𝑧-momentum DEPT Deposition time The available options include: <BLANK> SET *INITIAL_PWP_DEPTH Purpose: Initialize pore water pressure in solid elements where a non-hydrostatic profile is required. Card 1 1 2 3 4 5 6 7 8 Variable PID/PSID LC Type I I Default none none VARIABLE DESCRIPTION Part ID or Part Set ID for the_SET option Curve of pore water pressure head (length units) vs 𝑧-coordinate PID LC Remarks: This feature overrides the automatically calculated hydrostatic pressure profile. The points in the curve must be ordered with the most negative z-coordinate first – this order looks “upside-down” on the page. If a part has pore fluid but no *INITIAL_PWP_DEPTH is defined, the default initial pressure profile is hydrostatic. The available options include: <BLANK> SET *INITIAL Purpose: Initialize strain tensor for shell element. This option is primarily for multi- stage metal forming operations where the accumulated strain is of interest. These strain tensors are defined at the inner and outer integration points and are used for post-processing only. There is no interpolation with this option and the strains are defined in the global Cartesian coordinate system. The *DATABASE_EXTENT_BINA- RY flag STRFLG must be set to unity for this option to work. When OPTION is blank, users have the option to define strains at all integration points by providing nonzero NPLANE, NTHICK and setting INTOUT flag of *DATABASE_EXTENT_BINARY to either “STRAIN” or “ALL”. Card Sets. Define as many shell elements in this section as desired, one set of cards per element. The input is assumed to terminate when a new keyword is detected. Card 1 1 2 3 4 5 6 7 8 Variable EID NPLANE NTHICK Type I I I Default none none none When NPLANE and NTHICK are defined, include NPLANE × NTHICK cards below. For each through thickness point define NPLANE points. NPLANE should be either 1 or 4 corresponding to either 1 or 4 Gauss integration points. If four integration points are specified, they should be ordered such that their in plane parametric coordinates are at: √3 ⎜⎛− ⎝ , − √3 ⎟⎞ , 3 ⎠ ⎜⎛√3 ⎝ , − √3 ⎟⎞ , 3 ⎠ ⎜⎛√3 ⎝ , √3 ⎟⎞ , 3 ⎠ ⎜⎛− ⎝ √3 , √3 ⎟⎞ 3 ⎠ respectively. Strain Cards. When NPLANE and NTHICK are not defined or when the SET option is used, define two cards below, one for the inner integration point and the other for the outer integration point, respectively. Card 2 1 2 3 4 5 6 Variable EPSxx EPSyy EPSzz EPSxy EPSyz EPSzx Type F F F Default none none none F F F 0 8 7 T F 0. VARIABLE DESCRIPTION EID Element ID or shell element set ID when the SET option is used. NPLANE NTHICK EPSij T Number of in-plane integration points being output (not read when the SET option is used). Number of integration points through the thickness (not read when the SET option is used). Define the ij strain component. The strains are defined in the GLOBAL Cartesian system. Parametric coordinate of through thickness integration point between -1 and 1 inclusive. The availables options include: <BLANK> SET *INITIAL Purpose: Initialize strain tensor at element center. This option can be used for multi- stage metal forming operations where the accumulated strain is of interest. These strain tensors are defined at the element center and are used for post-processing only. The strains are defined in the global Cartesian coordinate system. The *DATA- BASE_EXTENT_BINARY flag STRFLG must be set to unity for this option to work. This capability is not available for the cohesive element since it is based on displacements, not strains. Card Sets. Define as many solid elements in this section as desired: one pair of cards per element. The input is assumed to terminate when a new keyword is detected. Element ID Cards. Card 1 1 2 3 4 5 6 7 8 Variable EID Type I Default none Strain Cards. Card 2 1 2 3 4 5 6 7 8 Variable EPSxx EPSyy EPSzz EPSxy EPSyz EPSzx Type F F F F F F VARIABLE DESCRIPTION EID EPSij Element ID or solid element set ID when the SET option is used. Define the ij strain component. The strains are defined in the GLOBAL cartesian system. *INITIAL_STRAIN_TSHELL Purpose: Initialize the strain tensors for thick shell elements.. Strain tensors are defined at the inner and outer integration points and are used for post-processing only. Strain tensors are defined in the global Cartesian coordinate system. The STRFLG flag on *DATABASE_EXTENT_BINARY must be set to unity for this option to work. Initialize as many elements as needed. Card Sets. For each element, include a set of cards 1, 2, and 3, where card 2 is for the inner layer and card 3 is for the outer layer. The input is assumed to terminate when a new keyword is detected Card 1 1 2 3 4 5 6 7 8 Variable EID Type I Default none Strain Cards. Card 2 is the strain at the inner layer. Card 3 is the strain at the outer layer. Cards 2, 3 1 2 3 4 5 6 7 8 Variable EPSxx EPSyy EPSzz EPSxy EPSyz EPSzx Type Default F 0 F 0 F 0 F 0 F 0 F 0 . VARIABLE DESCRIPTION EID EPSij Element ID. Define the ij strain component. The strains are defined in the GLOBAL Cartesian system. *INITIAL Purpose: Initialize stresses, plastic strains and history variables for Hughes-Liu beam elements, or the axial force, moment resultants and history variables for Belytschko- Schwer beam elements. Card Sets. Define as many beams in this section as desired. Each set consists of one Card 1 and several additional cards depending on variables NPTS, LARGE, NHISV, and NAXES. The input terminates when a new keyword (“*”) card is detected. Card 1 1 2 3 4 5 6 7 8 Variable EID RULE NPTS LOCAL LARGE NHISV NAXES Type I I I Default none none none I 0 I 0 I 0 I 0 Belytschko-Schwer Card for LARGE = 0. Additional card for the Belytschko-Schwer beam. Card 2 1 2 3 4 5 6 7 8 Variable F11 T11 M12 M13 M22 M23 PARM Type F F F F F F F Belytschko-Schwer Cards for LARGE = 1. Additional cards for the Belytschko- Schwer beam. Include as many cards as necessary to collect NHISV history variables. Card 2 1 2 3 4 5 6 7 8 9 10 Variable F11 Type F T11 F M12 M13 M22 F F *INITIAL_STRESS_BEAM Card 3 1 2 3 4 5 6 7 8 9 10 Variable M23 PARM HISV1 HISV2 HISV3 Type F F F F F Hughes-Liu Cards for LARGE = 0. Additional cards for the Hughes-Liu beam. Include NPTS additional cards, one per integration point. Card 2 1 2 3 4 5 6 7 8 Variable SIG11 SIG22 SIG33 SIG12 SIG23 SIG31 EPS Type F F F F F F F Hughes-Liu Cards for LARGE = 1. Additional cards for the Hughes-Liu beam. Include NPTS additional card sets, one per integration point. Include as many cards in one card set as necessary to collect NHISV history variables. Card 2 1 2 3 4 5 6 7 8 9 10 Variable SIG11 SIG22 SIG33 SIG12 SIG23 Type F F F F F . Card 3 1 2 3 4 5 6 7 8 9 10 Variable SIG31 Type F EPS F HISV1 HISV2 HISV3 F F Optional Local Axes Cards for NAXES = 12. Additional cards for definition of local axes values. These 12 values are internally used by LS-DYNA for the mapping between local beam element system and global coordinate system. They are automatically written to the dynain file if *INTERFACE_SPRINGBACK_LSDYNA or *CONTROL_- STAGED_CONSTRUCTION is used. Card 4 1 2 3 4 5 6 7 8 9 10 Variable AX1 Type F AX2 F AX3 F AX4 F AX5 F . Card 5 1 2 3 4 5 6 7 8 9 10 Variable AX6 Type F AX7 F AX8 F AX9 F AX10 F . Card 6 1 2 3 4 5 6 7 8 9 10 Variable AX11 AX12 Type F F VARIABLE DESCRIPTION EID Element ID RULE Integration rule type number: EQ.1.0: 1 × 1 Gauss quadrature, EQ.2.0: 2 × 2 Gauss quadrature (default beam), EQ.3.0: 3 × 3 Gauss quadrature, EQ.4.0: 3 × 3 Lobatto quadrature, EQ.5.0: 4 × 4 Gauss quadrature. NPTS Number of integration points. resultant beam element, NPTS = 1. For the Belytschko-Schwer *INITIAL_STRESS_BEAM DESCRIPTION LOCAL Coordinate system for stresses: EQ.0: Stress components are defined in the global coordinate system. EQ.1: Stress components are defined in the local beam system. In the local system components SIG22, SIG33, and SIG23 are set to 0.0. LARGE Format size: EQ.0: off, EQ.1: on. Each field is twice as long for higher precision. NHISV Number of additional history variables. Only available for LARGE = 1. NAXES Number of variables giving beam local axes (0 or 12) F11 T11 M12 M13 M22 M23 Axial force resultant along local beam axis 1 Torsional moment resultant about local beam axis 1 Moment resultant at node 1 about local beam axis 2 Moment resultant at node 1 about local beam axis 3 Moment resultant at node 2 about local beam axis 2 Moment resultant at node 2 about local beam axis 3 PARM Generally not used. SIGij EPS Define the ij stress component Effective plastic strain HISVn Define the nth history variable AXn The nth local axes value Available options include: <BLANK> SET *INITIAL Purpose: Initialize solid element stresses where stress is a function of depth. Card 1 1 2 3 4 Variable PID/PSID RO_G ZDATUM KFACT Type I F F F 5 LC I 6 7 8 LCH LCK0 I I Default none none none 0.0 none none none VARIABLE DESCRIPTION PID/PSID Part ID or Part Set ID for the SET option RO_G Stress per unit elevation above datum, which is usually 𝜌𝑔 = density × gravity. ZDATUM 𝑧-coordinate of datum KFACT 𝑥 and 𝑦-stresses = KFACT × 𝑧-stress Optional curve of stress vs z-coordinate (ZDATUM is ignored with this option) Optional curve of horizontal stress versus z-coordinate (KFACT is ignored with this option) Optional curve of K0 (ratio of horizontal_stress/vertical_stress) versus 𝑧-coordinate. KFACT and LCH are ignored with this option. The 𝑥-axis of the curve is the 𝑧-coordinate, the 𝑦-axis is K0. LC LCH LVK0 Remarks: With this keyword stress is calculated according to, σz = RO G × (Zelement − ZDATUM). To generate compressive stresses, the datum should be above the highest element. For instance, this is usually at the surface of the soil in geotechnics simulations. If the curve is present, it overrides RO_G and ZDATUM. Note that the points in the curve should be ordered with most negative 𝑧-coordinate first. First, select how the vertical stress as a function of 𝑧-coordinate will be defined (either RO_G and ZDATUM, or LC). Next, select how the horizontal stress will be defined (either a constant factor KFACT times the vertical stress; or a factor that varies with 𝑧- coordinate times the vertical stress using LCK0; or a curve of horizontal stress versus depth LCH). If pore water is present, the stresses input here are effective (soil skeleton stresses only). The pore water pressures will automatically be initialized to hydrostatic, or by *INI- TIAL_PWP_DEPTH or *BOUNDARY_PWP_TABLE if those cards are present. For a 2D problem (axisymmetric or plane strain), replace 𝑧 in above documentation with 𝑦. *INITIAL Purpose: Initialize the stress in solid elements that are included in a section definition (*DATABASE_CROSS_SECTION_option) to create a preload. The stress component in the direction normal to the cross-section plane is prescribed according to a curve. This option works with a subset of materials that are incrementally updated including the elastic, viscoelastic, and elastoplastic materials. Rubbers, foams, and materials that are combined with equations-of-state cannot be initialized by this approach, except as noted in Remark #3. Card 1 1 2 3 4 5 6 7 8 Variable ISSID CSID LCID PSID VID IZSHEAR Type I I I I I Default none none none none none I 0 VARIABLE DESCRIPTION ISSID CSID LCID PSID VID Section stress initialization ID. Cross-section ID. See *DATABASE_CROSS_SECTION. Load curve ID defining preload stress versus time. When the load curve ends or goes to zero, the initialization is assumed to be completed. See Remark 2. Part set ID. Vector ID defining the direction normal to the cross section. This vector must be defined if *DATABASE_CROSS_SECTION_SET is used to define the cross section. If the cross section is defined using the PLANE option, the normal used in the definition of the plane is used if VID is left undefined. IZSHEAR Shear stress flag: EQ.0: Shear stresses are prescribed as zero during the time the curve is acting to prescribe normal stress. EQ.1: Shear stresses are allowed to develop during the time the curve is acting to prescribe normal stress. *INITIAL_STRESS_SECTION 1. To achieve convergence during explicit dynamic relaxation, the application of the damping options is very important. If contact is active, contact damping is recommended with a value between 10-20 percent. Additional damping, via the option DAMPING_PART_STIFFNESS also speeds convergence where a coefficient of 0.10 is effective. If damping is not used, convergence may not be possible. 2. When defining the load curve, LCID, a ramp starting at the origin should be used to increase the stress to the desired value. The time duration of the ramp should produce a quasi-static response. When the end of the load curve is reached, or when the value of the load decreases from its maximum value, the initialization stops. If the load curve begins at the desired stress value, i.e., no ramp, convergence will take much longer, since the impulsive like load created by the initial stress can excite nearly every frequency in the structural system where stress is initialized. 3. This option currently applies only to materials that are incrementally updated. Hyperelastic materials and materials that require an equation-of-state are not currently supported. However, materials 57, 73, and 83 can be initialized with this approach. 4. Solid elements types 1, 2, 3, 4, 9, 10, 13, 15, 16, 17, and 18 are supported. ALE elements are not supported. Available options include: <BLANK> SET *INITIAL Purpose: Initialize stresses, history variables, and the effective plastic strain for shell elements. Materials that do not use an incremental formulation for the stress update may not be initializable with this card. Card Sets per Element. Define as many shell elements or shell element sets in this section as desired. The input is assumed to terminate when a new keyword (“*”) card is detected. Element Card. Card 1 1 2 3 4 5 6 7 8 Variable EID/SID NPLANE NTHICK NHISV NTENSR LARGE NTHINT NTHHSV Type I I I Default none none none I 0 I 0 I 0 I 0 I 0 Ordering of Integration Points. For each through thickness point define NPLANE points. NPLANE should be either 1 or 4 corresponding to either 1 or 4 Gauss integration points. If four integration points are specified, they should be ordered such that their in plane parametric coordinates are at: √3 ⎜⎛− ⎝ , − √3 ⎟⎞ , 3 ⎠ ⎜⎛√3 ⎝ , − √3 ⎟⎞ , 3 ⎠ ⎜⎛√3 ⎝ , √3 ⎟⎞ , 3 ⎠ ⎜⎛− ⎝ √3 , √3 ⎟⎞ , 3 ⎠ respectively. It is not necessary for the location of the through thickness integration points to match those used in the elements which are initialized. The data will be interpolated by LS DYNA. Solid Mechanics Data Card for LARGE = 0. The following set of cards: “Stress Card” through “Tensor Cards.” Should be included NPLANE × NTHICK times (one set for each integration point). Stress Card. Additional Card for LARGE = 0. Card 2 Variable Type 1 T F 2 3 4 5 6 7 8 SIGXX SIGYY SIGZZ SIGXY SIGYZ SIGZX EPS F F F F F F F History Variable Cards. Additional Cards for LARGE = 0. Include as many cards as necessary to collect NHISV history variables. Card 3 1 2 3 4 5 6 7 8 Variable HISV1 HISV2 HISV3 HISV4 HISV5 HISV6 HISV7 HISV8 Type F F F F F F F F Tensor Cards. Additional card for LARGE = 0. Include as many cards as necessary to collect NTENSR entries. Tensor cards contain only 6 entries per card. Card 4 1 2 3 4 5 6 7 8 Variable TENXX TENYY TENZZ TENXY TENYZ TENZX Type F F F F F F Solid Mechanics Data Card for LARGE = 1. The following set of cards: “Stress Card 1” through “Tensor Cards.” Should be included NPLANE × NTHICK times (one set for each integration point). Stress Card 1. Additional Card for LARGE = 1. Card 2 1 2 3 4 5 6 7 8 9 10 Variable Type T F SIGXX SIGYY SIGZZ SIGXY F F F Stress Card 2. Additional Card for LARGE = 1. Card 3 1 2 3 4 5 6 7 8 9 10 Variable SIGYZ SIGZX Type F F EPS F History Variable Cards. Additional Cards for LARGE = 1. Include as many cards as necessary to collect NHISV history variables. Card 4 1 2 3 4 5 6 7 8 9 10 Variable HISV1 HISV2 HISV3 HISV4 HISV5 Type F F F F F Tensor Cards. Include as many pairs of Cards 5 and 6 as necessary to collect NTENSR entries. Note that Cards 5 and 6 must allows appear as pairs, and that Card 6 may include at most one value, as indicated below. Card 5 1 2 3 4 5 6 7 8 9 10 Variable TENXX TENYY TENZZ TENXY TENYZ Type F F F F F Card 6 1 2 3 4 5 6 7 8 9 10 Variable TENZX Type F Thermal Data Cards for LARGE = 1. For each element, thermal data cards come after the entire set of mechanical data cards. For each of the NTHINT thermal integration points, include the following set of cards. Thermal Time History Cards. Additional cards for LARGE = 1. Include as many cards as needed to collect all the of NTHHSV time history variables per thermal integration point. Card 7 1 2 3 4 5 Variable THHSV1 THHSV2 THHSV3 THHSV4 THHSV5 Type F F F F F VARIABLE DESCRIPTION EID/SID Element ID or shell set ID, see *SET_SHELL_… NPLANE Number of in plane integration points being output. NTHICK Number of integration points through the thickness. NHISV Number of additional history variables. NTENSR Number of components of tensor data taken from the element history variables stored. LARGE Format size. See cards above. EQ.0: off EQ.1: on T SIGij Parametric coordinate of through thickness integration point between -1 and 1 inclusive. Define the ij stress component. The stresses are defined in the GLOBAL cartesian system. EPS Effective plastic strain. HISVn TENij Define the nth history variable. Define the ijth component of the tensor taken from the history variables. The tensor is defined in the GLOBAL Cartesian system. Define enough lines to provide a total of NTENSOR components, stored six components per line. This applies to material 190 only. NTHINT Number of thermal integration points. VARIABLE NTHHSV DESCRIPTION Number of thermal history variables per thermal integration point. THHSVn nth history variable at the thermal integration point. *INITIAL_STRESS_SOLID_{OPTION} Available options include: <BLANK> SET Purpose: Initialize stresses and plastic strains for solid elements. This command is not applicable to hyperelastic materials or any material model based on a Total Lagrangian formulation. Furthermore, for *MAT_014 and any material that requires an equation- of-state (*EOS), the specified initial stresses are adjusted to be in accordance with the initial pressure calculated from the equation of state. Card Sets per Element. For this keyword, each data card set consists of an element or element set card and all of its corresponding data cards, both thermal and mechanical. For LARGE = 1, this can involve several (even tens of) cards per set. Include cards for as many solid elements or solid element sets as desired. The input is assumed to terminate when a new keyword (“*”) card is detected. Card 1 1 2 3 4 5 6 7 8 Variable EID/SID NINT NHISV LARGE IVEFLG IALEGP NTHINT NTHHSV Type I I Default none none I 0 I 0 I 0 I 0 I 0 I 0 Ordering of Integration Points. NINT may be 1, 8, or 14 for hexahedral solid elements, depending on the element formulation. If eight Gauss integration points are specified, they should be ordered such that their parametric coordinates are located at: , − , − , − , − √3 √3 √3 ⎜⎛− ⎝ ⎜⎛√3 ⎝ √3 ⎟⎞ , 3 ⎠ √3 ⎟⎞ , 3 ⎠ respectively. If eight points are defined for 1 point LS-DYNA solid elements, the average value will be taken. √3 ⎟⎞ , 3 ⎠ √3 ⎟⎞ , 3 ⎠ ⎜⎛√3 ⎝ ⎜⎛√3 ⎝ √3 ⎟⎞ , 3 ⎠ √3 ⎟⎞ , 3 ⎠ √3 ⎟⎞ , 3 ⎠ ⎜⎛√3 ⎝ √3 3 ⎠ ⎜⎛− ⎝ ⎜⎛− ⎝ ⎜⎛− ⎝ √3 √3 √3 √3 √3 √3 √3 √3 √3 ⎟⎞, , − , − , − , − , , , , , , , , NINT may be 1, 4, or 5 for tetrahedral solid elements, depending on the element formulation and NIPTETS in *CONTROL_SOLID. NINT may be 1 or 2 for pentahedral solid elements, depending on the element formulation. Solid Mechanics Data Card for LARGE = 0. Stress Card. Additional Card for LARGE = 0. This card should be included NINT times (one for each integration point). Card 2 1 2 3 4 5 6 7 8 Variable SIGXX SIGYY SIGZZ SIGXY SIGYZ SIGZX EPS Type F F F F F F F Mechanical Data Cards for LARGE = 1. The following set of cards “Stress Card 1” through “Additional History Cards.” Should be included NINT times (one set for each integration point). Stress Card 1. Additional cards for LARGE = 1. Card 2 1 2 3 4 5 6 7 8 9 10 Variable SIGXX SIGYY SIGZZ SIGXY SIGYZ Type F F F F F Stress Card 2. Additional cards for LARGE = 1. Card 3 1 2 3 4 5 6 7 8 9 10 Variable SIGZX Type F EPS F HISV1 HISV2 HISV3 F F Additional History Cards. Additional cards for LARGE = 1. If NHISV > 3 define as many additional cards as necessary. NOTE: the value of IVEFLG can affect the number of history variables on these cards. Card 4 1 2 3 4 5 6 7 8 9 10 Variable HISV1 HISV2 HISV3 HISV4 HISV5 Type F F F F F Thermal Data Cards for LARGE = 1. For each element, thermal data cards come after the entire set of mechanical data cards. For each of the NTHINT thermal integration points, include the following set of cards. Thermal Time History Cards. Additional cards for LARGE = 1. Include as many cards as needed to capture all the of NTHHSV time history variables per thermal integration point. Card 5 1 2 3 4 5 6 7 8 9 10 Variable THHSV1 THHSV2 THHSV3 THHSV4 THHSV5 Type F F F F F VARIABLE DESCRIPTION EID/SID Element ID or solid set ID, see *SET_SOLID_... NINT NHISV LARGE Number of integration points (should correspond to the solid element formulation). Number of additional history variables, which is typically equal to the number of history variables stored at the integration point + IVEFLG. Format size, if zero, NHISV must also be set to zero (this is the format used by LS-DYNA versions 970 and earlier) and, if set to 1, a larger format is used and NHISV is used. VARIABLE DESCRIPTION IVEFLG Initial Volume/energy flag (only used in large format) EQ.0: last history variable is used as normal, EQ.1: last history variable is used as the initial volume of the element. One additional history variable is required if IVFLG = 1 EQ.2: last two history variables are used to define the initial volume and the internal energy per unit initial volume. Two additional history variables must be allocated, see NHISV above, if IVFLG = 2. If the initial volume is set to zero, the actual element volume is used. The ALE multi-material group (AMMG) ID; only if the element is of ALE multi-material formulation (ELEFORM = 11). In this case, each AMMG has its own sets of stress and history variables so we must specify to which AMMG the stress data are assigned. For mixed elements, multiple cards are needed to complete the stress initialization in this element as each AMMG needs to have its own set of stress data. EQ.0: Assuming the element is fully filled by the AMMG that the element part belongs to. Please refer to *ALE_MUL- TI-MATERIAL_GROUP card. EQ.n: Assigning the stress to nth AMMG in that element. Define the ijth stress component. Stresses are defined in the GLOBAL Cartesian system. Effective plastic strain Define (𝑁𝐻𝑆𝑉 + 𝐼𝑉𝐸𝐹𝐿𝐺) history variables. IALEGP SIGij EPS HISVi NTHINT Number of thermal integration points NTHHSV Number of thermal history variables per thermal integration point THHSVn nth thermal time history variable Remarks: 1. The elastic material model for cohesive elements is a total Lagrangian formulation, and the initial stress will therefore be ignored for it. *INITIAL_STRESS_SPH Purpose: Initialize stresses and plastic strains for SPH elements. This command is not applicable to hyperelastic materials or any material model based on a Total Lagrangian formulation. For *MAT_005, *MAT_014, and any material that requires an equation-of- state (*EOS), the initialized stresses are deviatoric stresses, not total stresses. Element Cards. Define as many SPH elements in this section as desired. The input is assumed to terminate when a new keyword is detected. Card 1 1 2 3 4 5 6 7 8 Variable EID SIGXX SIGYY SIGZZ SIGXY SIGYZ SIGZX EPS Type I F F F F F F F Default none none none none none none none none VARIABLE DESCRIPTION EID SIGij SPH particle ID Define the ijth stress component. Stresses are defined in the GLOBAL Cartesian system. EPS Effective plastic strain. *INITIAL Purpose: Initialize stresses and plastic strains for thick shell elements. Card Sets per Element. Define as many thick shell elements in this section as desired. The input is assumed to terminate when a new keyword is detected. Card 1 1 2 3 4 5 6 7 8 Variable EID NPLANE NTHICK NHISV LARGE Type I I I Default none none none I 0 I 0 Ordering of Integration Points. For each through thickness point define NPLANE points. NPLANE should be either 1 or 4 corresponding to either 1 or 4 Gauss integration points. If four integration points are specified, they should be ordered such that their in plane parametric coordinates are at: √3 ⎜⎛− ⎝ , − √3 ⎟⎞ , 3 ⎠ ⎜⎛√3 ⎝ , − √3 ⎟⎞ , 3 ⎠ ⎜⎛√3 ⎝ , √3 ⎟⎞ , 3 ⎠ ⎜⎛− ⎝ √3 , √3 ⎟⎞ 3 ⎠ respectively. It is not necessary for the location of the through thickness integration points to match those used in the elements which are initialized. The data will be interpolated by LS DYNA. Data Card for LARGE = 0. The following set of cards “Stress Card” and “History Cards.” Should be included NPLANE × NTHICK times (one set for each integration point). Stress Card. Additional card for LARGE = 0. Card 2 Variable Type 1 T F 2 3 4 5 6 7 8 SIGXX SIGYY SIGZZ SIGXY SIGYZ SIGZX EPS F F F F F F F History Cards. Additional Card for LARGE = 0. Include as many History Cards as needed to define all NHIST history variables. Optional 1 2 3 4 5 6 7 8 Variable HISV1 HSIV2 HSIV3 HSIV4 HSIV5 HSIV6 HSIV7 HSIV8 Type F F F F F F F F Data Card for LARGE = 1. The following set of cards “Stress Cards” and “History Cards.” Should be included NPLANE × NTHICK times (one set for each integration point). Stress Card 1. Additional card for LARGE = 1. Card 2 1 2 3 4 5 6 7 8 9 10 Variable Type T F SIGXX SIGYY SIGZZ SIGXY F F F F Stress Card 2. Additional card for LARGE = 3. Card 3 1 2 3 4 5 6 7 8 9 10 Variable SIGYZ SIGZX Type F F EPS History Cards. Additional Card for LARGE = 1. Include as many History Cards as needed to define all NHIST history variables. Optional 1 2 3 4 5 6 7 8 9 10 Variable HISV1 HISV2 HISV3 HISV4 HISV5 Type F F F F F VARIABLE DESCRIPTION EID Element ID NPLANE Number of in plane integration points. NTHICK Number of integration points through the thickness. T Parametric coordinate of through thickness integration point between -1 and 1 inclusive. NHISV Number of additional history variables. LARGE Format size. See keywords above. EQ.0: off EQ.1: on SIGij Define the ij stress component. The stresses are defined in the GLOBAL Cartesian system. EPS Effective plastic strain Available options include: NODE SET *INITIAL_TEMPERATURE Purpose: Define initial nodal point temperatures using nodal set ID’s or node numbers. These initial temperatures are used in a thermal only analysis or a coupled thermal/structural analysis. See also *CONTROL_THERMAL_SOLVER, *CONTROL_- THERMAL_TIMESTEP, and CONTROL_THERMAL_NONLINEAR. For thermal loading in a structural only analysis, see *LOAD_THERMAL_OPTION. Node/Node set Cards. Include one card for each node or node set. This input ends at the next keyword (“*”) keyword. Card 1 1 2 3 4 5 6 7 8 Variable NSID/NID TEMP LOC Type I I Default none 0. I 0 Remark 1 VARIABLE DESCRIPTION NSID/NID Nodal set ID or nodal point ID, see also *SET_NODES: EQ.0: all nodes are included (set option only). TEMP Temperature at node or node set. LOC For a thick thermal shell, the temperature will be applied to the surface identified by LOC, See parameter, THSHEL, on the *CONTROL_SHELL keyword. EQ.-1: lower surface of thermal shell element EQ.0: middle surface of thermal shell element EQ.1: upper surface of thermal shell element *INITIAL 1. This keyword can be used to define initial nodal point temperatures for SPH particles by using nodal set ID’s or node numbers from SPH particles. *INITIAL_VEHICLE_KINEMATICS Purpose: Define initial kinematical information for a vehicle. In its initial orientation, the vehicle’s yaw, pitch, and roll axes must be aligned with the global axes. Successive simple rotations are taken about these body fixed axes. Card 1 1 2 Variable GRAV PSID Type I I 3 XO F Default none none 0. 4 YO F 0. 5 ZO F 0. 6 XF F 0. 7 YF F 0. 8 ZF F 0. Card 2 Variable 1 VX Type F Default 0. 2 VY F 0. 3 VZ F 0. Card 3 1 2 3 4 5 6 7 8 AAXIS BAXIS CAXIS I 0 4 I 0 5 I 0 6 7 8 Variable AANG BANG CANG WA WB WC Type F Default 0. F 0. F 0. F 0. F 0. F 0. gravity roll yaw pitch Figure 23-3. The vehicle pictured is to be oriented with a successive rotation sequence about the yaw, pitch, and roll axes, respectively. Accordingly, AAXIS = 3, BAXIS = 1, and CAXIS = 2. The direction of gravity is given by GRAV = -3. VARIABLE DESCRIPTION GRAV Gravity direction code. EQ.1: Global +𝑥 direction. EQ.-1: Global −𝑥 direction. EQ.2: Global +𝑦 direction. EQ.-2: Global −𝑦 direction. EQ.3: Global +𝑧 direction. EQ.-3: Global −𝑧 direction. Note: this must be the same for all vehicles present in the model. PSID Part set ID. XO YO ZO XF YF ZF VX 𝑥-coordinate of initial position of mass center. 𝑦-coordinate of initial position of mass center. 𝑧-coordinate of initial position of mass center. 𝑥-coordinate of final position of mass center. 𝑦-coordinate of final position of mass center. 𝑧-coordinate of final position of mass center. global 𝑥-component of mass center velocity. VY VZ *INITIAL_VEHICLE_KINEMATICS DESCRIPTION global 𝑦-component of mass center velocity. global 𝑧-component of mass center velocity. AAXIS First rotation axis code. EQ.1: Initially aligned with global 𝑥-axis. EQ.2: Initially aligned with global 𝑦-axis. EQ.3: Initially aligned with global 𝑧-axis. BAXIS CAXIS Second rotation axis code. Third rotation axis code. AANG Rotation angle about the first rotation axis (degrees). BANG CANG WA WB WC Rotation angle about the second rotation axis (degrees). Rotation angle about the third rotation axis (degrees). Angular velocity component (radian/second). Angular velocity component (radian/second). Angular velocity component (radian/second). for the 𝑥 body-fixed axis for the 𝑦 body-fixed axis for the 𝑧 body-fixed axis *INITIAL Purpose: Define initial nodal point velocities using nodal set ID’s. This may also be used for sets in which some nodes have other velocities. See NSIDEX below. Card 1 1 2 3 4 5 6 7 8 Variable NSID NSIDEX BOXID IRIGID ICID Type I Default none Remark 1 Card 2 Variable 1 VX Type F Default 0. I 0 2 VY F 0. I 0 3 VZ F 0. I 0 I 0 4 5 6 7 8 VXR VYR VZR F 0. F 0. F 0. Exempted Node Card. Additional card for NSIDEX > 0. Card 3 1 2 3 4 5 6 7 8 Variable VXE VYE VZE VXRE VYRE VZRE Type F Default 0. F 0. F 0. F 0. F 0. F 0. VARIABLE NSID DESCRIPTION Nodal set ID, see *SET_NODES, containing nodes for initial velocity: If NSID = 0 the initial velocity is applied to all nodes. NSIDEX BOXID IRIGID ICID VX VY VZ VXR VYR VZR VXE VYE *INITIAL_VELOCITY DESCRIPTION Nodal set ID, see *SET_NODES, containing nodes that are exempted from the imposed velocities and may have other initial velocities. All nodes in box which belong to NSID are initialized. Nodes Exempted nodes are outside the box are not initialized. initialized to velocities defined by VXE, VYE, and VZE below regardless of their location relative to the box. Option to overwrite rigid body velocities defined on *PART_IN- ERTIA and *CONSTRAINED_NODAL_RIGID_BODY_INERTIA cards. GE.1: part set ID, containing ID of parts to overwrite. Center of gravity of part must lie within box BOXID. If BOXID is not defined then all parts defined in the set are over- written. EQ.-1: Overwrite velocities for all *PART_INERTIA's and *CONSTRAINED_NODAL_RIGID_BODY_INERTIA's with a center of gravity within box BOXID. If BOXID is not defined then all are overwritten. EQ.-2: Overwrite velocities for all *PART_INERTIA's and *CONSTRAINED_NODAL_RIGID_BODY_INERTIA's. Local coordinate system ID. The initial velocity is specified in the local coordinate system if ICID is greater than zero. Furthermore, if ICID is greater than zero, *INCLUDE_TRANSFORM does not rotate the initial velocity values specificied by VX, VY, …, VZRE. Initial translational velocity in 𝑥-direction Initial translational velocity in 𝑦-direction Initial translational velocity in 𝑧-direction Initial rotational velocity about the 𝑥-axis Initial rotational velocity about the 𝑦-axis Initial rotational velocity about the 𝑧-axis Initial velocity in 𝑥-direction of exempted nodes Initial velocity in 𝑦-direction of exempted nodes VARIABLE DESCRIPTION Initial velocity in 𝑧-direction of exempted nodes Initial rotational velocity in 𝑥-direction of exempted nodes Initial rotational velocity in 𝑦-direction of exempted nodes Initial rotational velocity in 𝑧-direction of exempted nodes VZE VXRE VYRE VZRE Remarks: 1. This generation input must not be used with *INITIAL_VELOCITY_GENERA- TION keyword. 2. If a node is initialized on more than one input card set, then the last set input will determine its velocity. However, if the nodal velocity is also specified on a *INITIAL_VELOCITY_NODE card, then the velocity specification on this card will be used. 3. Unless the option IRIGID is specified rigid bodies, initial velocities given in *PART_INERTIA will overwrite generated initial velocities. The IRIGID option will cause the rigid body velocities specified on the *PART_INERTIA input to be overwritten. To directly specify the motion of a rigid body without using the keyword, *PART_INERTIA, which also requires the definition of the mass properties, use the keyword option, *INITIAL_VELOCITY_RIGID_BODY. 4. Nodes which belong to rigid bodies must have motion consistent with the translational and rotational velocity of the center of gravity (c.g.) of the rigid body. During initialization the rigid body translational and rotational rigid body momentum's are computed based on the prescribed nodal velocity field. From this rigid body momentum, the translational and rotational velocities of the nodal points are computed and reset to the new values. These new values may or may not be the same as the values prescribed for the nodes that make up the rigid body. Sometimes this occurs in single precision due to numerical round-off. If a problem like this occurs specify the velocity using the keyword: *INITIAL_VELOCITY_RIGID_BODY. 5. Mid-side nodes generated by *ELEMENT_SOLID_TET4TO10 will not be initialized since the node numbers are not known a priori to the user. Instead use *INITIAL_VELOCITY_GENERATION if you intend to initialize the veloci- ties of the mid-side nodes. Purpose: Define initial nodal point velocities for a node. *INITIAL_VELOCITY_NODE Card 1 Variable NID Type I 2 VX F Default none 0. 3 VY F 0. 4 VZ F 0. 5 6 7 8 VXR VYR VZR ICID F 0. F 0. F 0. I 0 VARIABLE DESCRIPTION NID Node ID VX VY VZ VXR VYR VZR ICID Initial translational velocity in 𝑥-direction Initial translational velocity in 𝑦-direction Initial translational velocity in 𝑧-direction Initial rotational velocity about the 𝑥-axis Initial rotational velocity about the 𝑦-axis Initial rotational velocity about the 𝑧-axis Local coordinate system ID. The specified velocities are in the local system if ICID is greater than zero. Furthermore, if ICID is greater than zero, *INCLUDE_TRANSFORM does not rotate the initial velocity values specificied by VX, VY, …, VZR. See Remarks on *INITIAL_VELOCITY card. *INITIAL Purpose: Define the initial translational and rotational velocities at the center of gravity (c.g.) for a rigid body or a nodal rigid body. This input overrides all other velocity input for the rigid body and the nodes which define the rigid body. Card 1 Variable PID Type I 2 VX F Default none 0. 3 VY F 0. 4 VZ F 0. 5 6 7 8 VXR VYR VZR ICID F 0. F 0. F 0. I 0 VARIABLE DESCRIPTION PID VX VY VZ VXR VYR VZR ICID Part ID of the rigid body or the nodal rigid body. Initial translational velocity at the c.g. in global 𝑥-direction. Initial translational velocity at the c.g. in global 𝑦-direction. Initial translational velocity at the c.g. in global 𝑧-direction. Initial rotational velocity at the c.g. about the global 𝑥-axis. Initial rotational velocity at the c.g. about the global 𝑦-axis. Initial rotational velocity at the c.g. about the global 𝑧-axis. Local coordinate system ID. The specified velocities are in the local system if ICID is greater than zero. Furthermore, if ICID is greater than zero, *INCLUDE_TRANSFORM does not transform the initial velocity values specificied by VX, VY, …, VZR. See remarks 3 and 4 on the *INITIAL_VELOCITY input description. *INITIAL_VELOCITY_GENERATION Purpose: Define initial velocities for rotating and translating bodies. NOTE: Rigid body velocities cannot be reinitialized after dynamic relaxation by setting PHASE=1 since rigid body velocities are always restored to the values that existed prior to dynamic relaxation. Reinitialization of velocities after dynamic relaxation is only availa- ble for nodal points of deformable bodies; therefore, if rigid bodies are present in the part set ID, this in- put should be defined twice, once for PHASE=0 and again for PHASE=1. Card 1 Variable 1 ID 2 3 STYP OMEGA Type I I F Default none none 0. Card 2 Variable 1 XC Type F Default 0. 2 YC F 0. 3 ZC F 0. 4 VX F 0. 4 NX F 0. 5 VY F 0. 5 NY F 0. VARIABLE DESCRIPTION 6 VZ F 0. 6 NZ F 0. 7 8 IVATN ICID I 0 7 I 0 8 PHASE IRIGID I 0 I 0 ID Part ID, part set ID, or node set ID. If zero, STYP is ignored, and all velocities are set. WARNING if IVATN = 0: If a part ID of a rigid body is specified only the nodes that belong to elements of the rigid body are initialized. Nodes defined under the keyword. Set initialized. *CONSTRAINED_EXTRA_NODES are not IVATN = 1 to initialize velocities of slaved nodes and parts. VARIABLE DESCRIPTION STYP Set type. See Remark 5. EQ.1: part set ID, see *SET_PART, EQ.2: part ID, see *PART, EQ.3: node set ID, see *SET_NODE. OMEGA Angular velocity about the rotational axis. VX VY VZ Initial translational velocity in 𝑥-direction . Initial translational velocity in 𝑦-direction . Initial translational velocity in 𝑧-direction . IVATN Flag for setting the initial velocities of slave nodes and parts: EQ.0: slaved parts are ignored. EQ.1: slaved parts and slaved nodes of the master parts will be assigned initial velocities like the master part. Local coordinate system ID. The specified translational velocities (VX, VY, VZ) and the direction cosines of the rotation axis (NX, NY, NZ) are in the global system if ICID = 0 and are in the local system if ICID is defined. Therefore, if ICID is defined, *INCLUDE_TRANSFORM does not transform (VX, VY, VZ) and (NX, NY, NZ). Global 𝑥-coordinate on rotational axis. Global 𝑦-coordinate on rotational axis. Global 𝑧-coordinate on rotational axis. 𝑥-direction cosine. If set to -999, NY and NZ are interpreted as the 1st and 2nd nodes defining the rotational axis, in which case the coordinates of node NY are used as XC, YC, ZC. If ICID is defined, the direction cosine, (NX, NY, NZ), is projected along coordinate system ICID to yield the direction cosines of the rotation axis only if NX ≠ -999. 𝑦-direction cosine or the 1st node of the rotational axis when NX = -999. ICID XC YC ZC NX NY NZ *INITIAL_VELOCITY_GENERATION DESCRIPTION 𝑧-direction cosine or the 2nd node of the rotational axis when NX = -999. PHASE Flag specifying phase of the analysis the velocities apply to: EQ.0: Velocities are applied immediately, EQ.1: Velocities are applied after reaching the start time, STIME, which is after dynamic relaxation, if active, is completed. See the keyword: *INITIAL_VELOCITY_- GENERATION_START_TIME. STIME defaults to zero. Controls hierarchy of initial velocities set with *INITIAL_VELOC- ITY_GENERATION versus those set with *PART_INERTIA / *CONSTRAINED_NODAL_RIGID_BODY_INERTIA when the commands conflict. EQ.0: *PART_INERTIA / *CONSTRAINED_NODAL_RIGID_- BODY_INERTIA controls initial velocities. EQ.1: *INITIAL_VELOCITY_GENERATION controls velocities. This option does not apply if STYP = 3. initial IRIGID Remarks: 1. Exclusions. This generation input must not be used with *INITIAL_VELOCI- TY or *INITIAL_VELOCITY_NODE options. 2. Order Dependence. The velocities are initialized in the order the *INITIAL_- VELOCITY_GENERATION input is defined. Later input via the *INITIAL_VE- LOCITY_GENERATION keyword may overwrite the velocities previously set. 3. Consistency for Rigid Body Nodes. Nodes which belong to rigid bodies must have motion consistent with the translational and rotational velocity of the rigid body. During initialization the rigid body translational and rotational rigid body momentum's are computed based on the prescribed nodal velocities. From this rigid body motion the velocities of the nodal points are computed and reset to the new values. These new values may or may not be the same as the values prescribed for the node. 4. SPH. SPH elements can be initialized using the STYP=3 option only. 5. Constrained Nodal Rigid Bodies. Part IDs of *CONSTRAINED_NODAL_- RIGID_BODYs that do not include the INERTIA option are not recognized by the code in the case of STYP=1 or 2. Use STYP=3 (a node set ID) when initializ- ing velocity of such nodal rigid bodies. *INITIAL_VELOCITY_GENERATION_START_TIME Purpose: Define a time to initialize velocities after time zero. Time zero starts after dynamic relaxation if used for initialization. Card 1 1 2 3 4 5 6 7 8 Variable STIME Type F Default 0.0 VARIABLE DESCRIPTION STIME Start time. Remarks: 1. Only one *INITIAL_VELOCITY_GENERATION_START_TIME can be specified. Multiple start times are not allowed. 2. All *INITIAL_VELOCITY_GENERATION commands adhere to the start time provided the requirement is met that at least one of those commands has PHASE set to 1. 3. When *INITIAL_VELOCITY_GENERATION_START_TIME is active, nodes that are not part of the initial velocity generation definitions will be re- initialized with velocities as they were at 𝑡 = 0. Available options include: PART SET *INITIAL Purpose: Define initial voided part set ID’s or part numbers. This command can be used only when ELFORM = 12 in *SECTION_SOLID. Void materials cannot be created during the calculation. Fluid elements which are evacuated, e.g., by a projectile moving through the fluid, during the calculation are approximated as fluid elements with very low densities. The constitutive properties of fluid materials used as voids must be identical to those of the materials which will fill the voided elements during the calculation. Mixing of two fluids with different properties is not permitted with this option. Card 1 1 2 3 4 5 6 7 8 Variable PSID/PID Type I Default none Remark 1 VARIABLE DESCRIPTION PSID/PID Part set ID or part ID, see also *SET_PART: Remarks: This void option and multiple materials per element, see *ALE_MULTI-MATERIAL_- GROUP are incompatible and cannot be used together in the same run. *INITIAL_VOLUME_FRACTION_OPTION Available option: NALEGP Purpose: Define initial volume fractions of different materials in multi-material ALE elements. Without NALEGP option, the keyword allows up to 7 ALE multi-material groups. The NALEGP option adds in an additional card immediately after the keyword to let users input the number of ALE multi-material groups to be read in for each element. Format without NALEGP option: Card 1 1 2 3 4 5 6 7 8 Variable EID VF1 VF2 VF3 VF4 VF5 VF6 VF7 Type I F F F F F F F Default none 0.0 0.0 0.0 0.0 0.0 0.0 0.0 Card 1 repeated multiple times. Each card for an ALE element volume fraction information. Format with NALEGP option: NALEGP Card. Additional card for the NALEGP keyword option. Optional 1 Variable NALEGP Type Card 1 1 2 3 4 5 6 7 8 Variable EID VF1 VF2 VF3 VF4 VF5 VF6 VF7 Type I F F F F F F F Default none 0.0 0.0 0.0 0.0 0.0 0.0 0.0 Card 1a 1 2 3 4 5 6 7 8 Variable VF8 VF9 VF10 VF11 VF12 VF13 VF14 VF15 Type I F F F F F F F Default none 0.0 0.0 0.0 0.0 0.0 0.0 0.0 … Card 1z 1 2 3 4 5 6 7 8 Variable VF(NGP-2) VF(NGP-1) VF(NGP) Type I F F Default none 0.0 0.0 Card 1 is continued by additional cards until all the NALEGP volume fractions for this element are listed. Card 1 and its continuation cards are repeated until all ALE elements are finished. VARIABLE DESCRIPTION EID VF1 VF2 Element ID. Volume fraction of multi-material group 1, AMMGID = 1. Volume fraction of multi-material group 2. Only needed in simulations with 3 material groups. Otherwise VF2 = 1 − VF1. *INITIAL_VOLUME_FRACTION DESCRIPTION VF3 VF4 VF5 VF6 VF7 Volume fraction of multi-material group 3, AMMGID = 3. Volume fraction of multi-material group 4, AMMGID = 4. Volume fraction of multi-material group 5, AMMGID = 5. Volume fraction of multi-material group 6, AMMGID = 6. Volume fraction of multi-material group 7, AMMGID = 7. VF(N) Volume fraction of multi-material group N, AMMGID = N. *INITIAL_VOLUME_FRACTION_GEOMETRY Purpose: This is a volume-filling command for defining the volume fractions of various ALE multi-material groups (AMMG) that initially occupy various spatial regions in an ALE mesh. This applies only to ELFORMs 11 and 12 in *SECTION_SOLID and ALE- FORM 11 in *SECTION_ALE2D. For ELFORM 12, AMMGID 2 is void. See Remark 2. Background ALE Mesh Card. Defines the background ALE mesh set & an AMMGID that initially fills it. Card 1 1 2 3 4 5 6 7 8 Variable FMSID FMIDTYP BAMMG NTRACE Type I Default none I 0 I 0 I 3 VARIABLE FMSID DESCRIPTION A background ALE (fluid) mesh SID to be initialized or filled with various AMMG’s. This set ID refers to one or more ALE parts. FMIDTYP ALE mesh set ID type: EQ.0: FMSID is an ALE part set ID (PSID). EQ.1: FMSID is an ALE part ID (PID). BAMMG NTRACE The background fluid group ID or ALE Multi-Material group ID (AMMGID) that initially fills all ALE mesh region defined by FMSID. Number of sampling points for volume filling detection. Typically NTRACE ranges from 3 to maybe 10 (or more). The higher it is, the finer the ALE element is divided so that small gaps between 2 Lagrangian shells may be filled in. See Remark 4. Pairs of Container Cards. For each container include one “Container Card” (Card a) and one geometry card (Card bi). Include as many pairs as desired. This input ends at the next keyword (“*”) card. Contained Card. Defines the container type and the AMMGID that fills the region defined by the container type. Card a 1 2 3 Variable CNTTYP FILLOPT FAMMG Type I Default none I 0 I none 7 8 4 VX F 0 5 VY F 0 6 VZ F 0 DESCRIPTION VARIABLE CNTTYP A “container” defines a Lagrangian surface boundary of a spatial region, inside (or outside) of which, an AMMG would fill up. CNTTYP defines the container geometry type of this surface boundary (or shell structure). EQ.1: The container geometry is defined by a part ID (PID) or a part set ID (PSID), where the parts should be defined by shell elements . EQ.2: The container geometry is defined by a segment set (SGSID). EQ.3: The container geometry is defined by a plane: a point and a normal vector. EQ.4: The container geometry is defined by a conical surface: 2 end points and 2 corresponding radii (in 2D see Remark 6). EQ.5: The container geometry is defined by a cuboid or rectangular box: 2 opposing end points, minimum to maximum coordinates. EQ.6: The container geometry is defined by a sphere: 1 center point, and a radius. VARIABLE FILLOPT FAMMG DESCRIPTION A flag to indicate which side of the container surface the AMMG is supposed to fill. The “head” side of a container sur- face/segment is defined as the side pointed to by the heads of the normal vectors of the segments (“tail” side refers to opposite direction to “head”). See Remark 5. EQ.0: The “head” side of the geometry defined above will be filled with fluid (default). EQ.1: The “tail” side of the geometry defined above will be filled with fluid. This defines the fluid group ID or ALE Multi-Material group ID (AMMGID) which will fill up the interior (or exterior) of the space defined by the “container”. The order of AMMGIDs is determined by the order in which they are listed under *ALE_MULTI-MATERIAL_- GROUP card. For example, the first data card under the *ALE_- MULTI-MATERIAL_GROUP keyword defines the multi-material group with ID (AMMGUD) 1, the second data card defined AM- MGID = 2 and so on. LT.0: | | FAMMG *SET_MULTI- MATERIAL_GROUP_LIST id listing pairs of group IDs. For each pair, the 2nd group replaces the first one in the “container”. is a VX VY VZ Initial velocity in the global 𝑥-direction for this AMMGID. Initial velocity in the global 𝑦-direction for this AMMGID. Initial velocity in the global 𝑧-direction for this AMMGID. Part/Part Set Container Card. Additional card for CNTTYP = 1. Card b1 1 2 3 4 5 6 7 8 Variable SID STYPE NORMDIR XOFFST Type I Default none I 0 I 0 F 0.0 Remark obsolete VARIABLE SID DESCRIPTION A Set ID pointing to a part ID (PID) or part set ID (PSID) of the Lagrangian shell element structure defining the “container” geometry to be filled . SSTYPE Set ID type: EQ.0: Container SID is a Lagrangian part set ID (PSID). EQ.1: Container SID is a Lagrangian part ID (PID). NORMDIR Obsolete . XOFFST Absolute length unit for offsetting the fluid interface from the nominal fluid interface LS-DYNA would otherwise define by default. This parameter only applies to GEOTYPE = 1 (4th column) and GEOTYPE = 2 (3rd column). This is applicable to cases in which high pressure fluid is contained within a container. The offset allows LS-DYNA time to prevent leakage. In general, this may be set to roughly 5-10% of the ALE elm width. It may be important only for when ILEAK is turned ON to give the code time to "catch" the leakage. If ILEAK is not ON, this may not be necessary. Segment Set Container Card. Additional card for CNTTYP = 2. Card b2 1 2 3 4 5 6 7 8 Variable SGSID NORMDIR XOFFST Type I Default none I 0 F 0.0 Remark obsolete VARIABLE DESCRIPTION SGSID Segment Set ID defining the “container”, see *SET_SEGMENT. NORMDIR Obsolete . XOFFST Absolute length unit for offsetting the fluid interface from the nominal fluid interface LSDYNA would otherwise define by default. This parameter only applies to GEOTYPE = 1 (4th column) and GEOTYPE = 2 (3rd column). This is applicable to cases in which high pressure fluid is contained within a container. The offset allows LS-DYNA time to prevent leakage. In general, this may be set to roughly 5-10% of the ALE elm width. It may be important only for when ILEAK is turned ON to give the code time to "catch" the leakage. If ILEAK is not ON, this may not be necessary. Plane Card. Additional card for CNTTYP = 3. Card b3 Variable 1 X0 Type F 2 Y0 F 3 Z0 F 4 5 6 7 8 XCOS YCOS ZCOS F F F Default none none none none none none VARIABLE DESCRIPTION X0, Y0, Z0 𝑥, 𝑦 and 𝑧 coordinate of a spatial point on the plane. XCOS, YCOS, ZCOS 𝑥, 𝑦 and 𝑧 direction cosines of the plane normal vector. The filling will occur on the side pointed to by the plane normal vector (or “head” side). Cylinder/Cone Container Card. Additional Card for CNTTYP = 4 . Card b4 Variable 1 X0 Type F 2 Y0 F 3 Z0 F 4 X1 F 5 Y1 F 6 Z1 F 7 R1 F 8 R2 F Default none none none none none none none none VARIABLE DESCRIPTION X0, Y0, Z0 𝑥, 𝑦 and 𝑧 coordinate of the center of the 1st base of the cone. X1, Y1, Z1 𝑥, 𝑦 and 𝑧 coordinate of the center of the 2nd base of the cone. R1 R2 Radius of the 1st base of the cone Radius of the 2nd base of the cone Rectangular Box Container Card. Additional Card for CNTTYP = 5. Card b5 Variable 1 X0 Type F 2 Y0 F 3 Z0 F 4 X1 F 5 Y1 F 6 Z1 F 7 8 LCSID I Default none none none none none none none VARIABLE DESCRIPTION X0, Y0, Z0 Minimum 𝑥, 𝑦 and 𝑧 coordinates of the box. VARIABLE DESCRIPTION X1, Y1, Z1 Maximum 𝑥, y and 𝑧 coordinates of the box. LCSID Local coordinate system ID, if defined, the box is aligned with the local coordinate system instead of global coordinate system. Please see *DEFINE_COORDINATE_ for details. Sphere Container Card. Additional card for CNTTYP = 6. 5 6 7 8 Card b6 Variable 1 X0 Type F 2 Y0 F 3 Z0 F 4 R0 F Default none none none none VARIABLE DESCRIPTION X0, Y0, Z0 𝑥, 𝑦 and 𝑧 coordinate of the center of the sphere. R0 Radius of the sphere Remarks: 1. Structure of Data Cards. After card 1 defining the basic mesh filled by certain fluid group (AMMGID), each “filling action” will require 2 additional lines of input (cards a, and b#, where # is the CNTTYP value). At the minimum there will be 3 cards required for this command (1, a, and b#) for 1 “filling action”. There can be one or more “filling actions” prescribed for each instance of this command. The “filling actions” take place in the prescribed order and the ef- fects are cumulative. Later filling actions will over-write the previous ones. Therefore any complex filling logic will require some planning. For example, the following card sequence, with 2 “filing actions”, is allowable: *INITIAL_VOLIME_FRACTION_GEOMTRY [Card 1] [Card a, CNTTYP = 1] [Card b1] [Card a, CNTTYP = 3] [Card b3] This sequence of cards prescribes a system of background ALE mesh with 2 “filing actions” to be executed. The 1st is a filling of a CNTTYP = 1, and the 2nd of CNTTYP = 3. “Card a” is required for all container geometry types (CNTTYP). “Card bi” defines the container actual geometry and corresponds to each of the CNTTYP choice. 2. Group IDs for ELFORM 12. If ELFORM=12, the single-material-and-void element forumation, is used in *SECTION_SOLID, then the non-void material is defaults to AMMG = 1 and the void to AMMG = 2. These multi-material groups are implied even though no *ALE_MULTI-MATERIAL_GROUP card is required. 3. Using Shells to Divide Space. A simple ALE background mesh (for example, a cuboid mesh) can be constructed enveloping some Lagrangian shell structure (or container). The ALE region inside this Lagrangian shell container may be filled with one multi-material group (AMMG1), and the outside region with another (AMMG2). This approach simplifies the mesh generation requirements for ALE material parts with complex geometries. 4. NTRACE. Default is NTRACE=3 in which case the total number is (2 × NTRACE + 1)3 = 73 This means an ALE element is subdivided into 7 × 7 × 7 regions. Each is to be filled in with the appropriate AMMG. An example of this application would be the filling of initial gas between multiple layers of Lagrangian airbag shell ele- ments sharing the same ALE element. 5. Interior/Exterior Fill Setting. To set which side of a container is to be filled: (1) define the shell (or segment) container with inward normal vectorsl; then (2) set the FILLOPT field on “Card a” to 0, corresponding to the head of the normal, for the interior, and to 1, corresponding to the tail of the normal, for the exteri- or. 6. Two Dimensional Geometry. If the ALE model is 2D (*SECTION_ALE2D instead of *SECTION_SOLID), CNTTYP=4 defines a quadrangle. In this case the fields which, in the 3D case define a cone, are interpreted as the corner co- ordinates of a clockwise defined (inward normal) quadrangle having the verti- ces: (X1, Y1 ), (X2, Y2), (X3, Y3), and (X4, Y4). The CNTYPE = 4 input fields X0, Y0, Z0, X1, Y1, Z1, R1, and R2 becomes X1, Y1, X2, Y2, X3, Y3, X4, and Y4 re- spectively. CNTTYP=6 should be used to fill a circle. Example: Consider a simple ALE model with ALE parts H1-H5 (5 AMMGs possible) and 1 Lagrangian shell (container) part S6. Only parts H1 and S6 initially have their meshes defined. We will perform 4 “filling actions”. The volume filling results after each step will be shown below to clarify the concept used. The input for the volume filling looks like this. $...|....1....|....2....|....3....|....4....|....5....|....6....|....7....|....8 $ H1 = AMMG 1 = fluid 1 initially occupying whole ALE mesh= background mesh $ H5 = AMMG 5 = fluid 5 fills below a plane = filling action 1 = CNTTYP=3 $ H2 = AMMG 2 = fluid 2 fills outside S5 = filling action 2 = CNTTYP=1 $ H3 = AMMG 3 = fluid 3 fills inside a cone = filling action 3 = CNTTYP=4 $ H4 = AMMG 4 = fluid 4 fills inside a box = filling action 4 = CNTTYP=5 $ S6 = Lagrangian shell container $...|....1....|....2....|....3....|....4....|....5....|....6....|....7....|....8 *ALE_MULTI-MATERIAL_GROUP 1 1 2 1 3 1 4 1 5 1 *INITIAL_VOLUME_FRACTION_GEOMETRY $ The 1st card fills the whole pid H1 with AMMG 1=background ALE mesh $ FMSID FMIDTYP BAMMG <=== card 1: background fluid 1 1 1 $ filling action 1 = AMMG 5 fill all elms below a plane $ CNTTYPE FILLOPT FILAMMGID <=== card a : container: CNTTYPE=3=plane 3 0 5 $ X0, Y0, Z0, NX, NY, NZ <=== card b-3: details on container =plane 25.0,20.0, 0.0, 0.0,-1.0,0.0 $ filling action 2: AMMG 2 fills OUTSIDE (FILLOPT=1) shell S6 (inward normals); $ CNTTYPE FILLOPT FAMMG <== card a : container #1; FILLOPT=1=fill tail 1 1 2 $ SETID SETTYPE NORMDIR <== card b-1: details on container #1 6 1 0 $ filling action 3 = AMMG 3 fill all elms inside a CONICAL region $ CNTTYPE FILLOPT FAMMG CNTTYP = 4 = Container = conical region 4 0 3 $ X1 Y1 Z1 X2 Y2 Z2 R1 R2 25.0 75.0 0.0 25.0 75.0 1.0 8.0 8.0 $ filling action 4 = AMMG 4 fill all elms inside a BOX region $ CNTTYPE FILLOPT FFLUIDID : CNTTYP=5 = "BOX" 5 0 4 $ XMIN YMIN ZMIN XMAX YMAX ZMAX 65.0 35.0 0.0 85.0 65.0 1.0 $...|....1....|....2....|....3....|....4....|....5....|....6....|....7....|....8 Before the 1st “filling action” the whole ALE mesh of part H1 is filled with AMMG 1 (white). After the 1st “filling action”, AMMG 5 fills below the specified plane. After the 1st and 2nd “filling actions”, it fills outside the shell (S6) with AMMG 2. After the 1st, 2nd and 3rd “filling actions”, it fills in the analytical sphere with AMMG 3. After the 1st, 2nd, 3rd and 4th “filling actions”, it fills in the analytical box with AMMG 4. In this section the user defined integration rules for beam and shell elements are specified. IRID refers to integration rule identification number on *SECTION_BEAM and *SECTION_SHELL cards respectively. Quadrature rules in the *SECTION_SHELL and *SECTION_BEAM cards need to be specified as a negative number. The absolute value of the negative number refers to user defined integration rule number. Positive rule numbers refer to the built in quadrature rules within LS-DYNA. The keyword cards in this section are: *INTEGRATION_BEAM *INTEGRATION_SHELL *INTEGRATION_BEAM Purpose: To support user defined through the thickness integration rules for the beam element. Card 1 1 Variable IRID Type I Default none 2 NIP I 0 3 RA F 0.0 4 ICST I 0 5 K I 0 6 7 8 Standard Cross-Section Card. Additional card for ICST > 0. Card Variable 1 D1 Type F 2 D2 F 3 D3 F 4 D4 F 5 6 SREF TREF F F 7 D5 F 8 D6 F Default none none none none 0.0 0.0 none none Quadrature Cards. Include NIP additional cards below for NIP ≠ 0. Card Variable Type 1 S F 2 T F 3 WF 4 PID F I 5 6 7 8 VARIABLE IRID DESCRIPTION Integration rule ID. IRID refers to IRID on *SECTION_BEAM card. NIP Number of integration points, see also ICST. st tt Thicknesses defined on beam cross-section cards Relative Area = st × tt Figure 24-1. Definition of relative area for user defined integration rule. VARIABLE RA DESCRIPTION Relative area of cross section, i.e., the actual cross-sectional area divided by the area defined by the product of the specified thickness in the s direction and the thickness in the t direction. See also ICST below and Figure 24-1. ICST Standard cross section type, ICST. If this type is nonzero then NIP and the relative area above should be input as zero. See shapes in Figure 24-2 following Remarks. EQ.01: I-Shape EQ.02: Channel EQ.03: L-shape EQ.04: T-shape EQ.05: Tubular box EQ.06: Z-Shape EQ.07: Trapezoidal EQ.08: Circular EQ.09: Tubular EQ.10: I-Shape 2 EQ.11: Solid Box EQ.12: Cross EQ.13: H-Shape EQ.14: T-Shape 2 EQ.15: I-Shape 3 EQ.16: Channel 2 EQ.17: Channel 3 EQ.18: T-Shape 3 EQ.19: Box-Shape 2 EQ.20: Hexagon EQ.21: Hat-Shape EQ.22: Hat-Shape 2 A1 A2 A3 A12 A11 A10 A5 A4 A6 A7 A8 A9 Figure 24-2. Definition of integration points for user defined integration rule. VARIABLE DESCRIPTION K Integration refinement parameter for standard cross section types. Select an integer ≥ 0. See Figure below. D1-D6 Cross-section dimensions. See Figure below. SREF TREF S T WF sref, location of reference surface normal to s, for the Hughes-Liu beam only. This option is only useful if the beam is connected to a shell or another beam on its outer surface. Overrides NSLOC in *SECTION_BEAM even if SREF = 0. tref, location of reference surface normal to t, for the Hughes-Liu beam only. This option is only useful if the beam is connected to a shell or another beam on its outer surface. Overrides NTLOC in *SECTION_BEAM even if TREF = 0. Normalized s coordinate of integration point, −1 ≤ 𝑠 ≤ 1. Normalized t coordinate of integration point, −1 ≤ 𝑡 ≤ 1. Weighting factor, Ari integration point divided by actual cross sectional area the area associated with the , i.e., 𝐴𝑟𝑖 = 𝐴𝑖 ⁄ , see Figure 24-1. DESCRIPTION Optional PID, used to identify material properties for this integration point. If zero, the “master” PID (referenced on *ELEMENT) will be used. This feature will be available in release 3 of version 971. VARIABLE PID Remarks: The input for standard beam section types is defined below. In following figures the dimensions are shown on the left and the location of the integration points are shown on the right. If a quantity is not defined in the sketch, then it should be set to zero in the input. The input quantities include: D1 - D6 = Dimensions of section k = Integration refinement parameter ( an integer GE. 0) sref = location of reference surface normal to s, Hughes-Liu beam only tref = location of reference surface normal to t, Hughes-Liu beam only D3 D1 (a) D2 D4 2k+4 2k+3 4k+7 6k+9 4k+6 15 16 17 18 19 20 21 10 11 12 13 14 (b) (c) Figure 24-3. Type 1: I-Shape. (a) Cross section geometry. (b) Integration point numbering. (c) Example for k = 2. D4 D3 D1 (a) D2 2k+7 3k+9 k+4 k+3 2k+6 11 12 13 14 15 10 (b) (b) Figure 24-4. Type 2: Channel. (a) Cross section geometry. (b) Integration point numbering. (c) Example for k = 2. D4 D3 K+2 D2 K+3 K+4 2K+5 D1 (a) (b) (c) Figure 24-5. Type 3: L-shape. (a) Cross section geometry. (b) Integration point numbering. (c) Example for k = 2. D3 D1 (a) D4 D2 k+2 k+3 k+4 2k+6 2k+5 3 4 4k+9 (b) 6 7 8 9 10 11 12 13 14 15 16 17 (c) Figure 24-6. Type 4: T-shape. (a) Cross section geometry. (b) Integration point numbering. (c) Example for k = 2. D3 D2 D1 (a) 2k+7 k+3 3k+8 D4 3k+7 k+4 4k+8 2k+6 11 12 13 14 15 16 10 (b) (c) Figure 24-7. Type 5: Box-shape. (a) Cross section geometry. (b) Integration point numbering. (c) Example for k = 2. D4 D3 D2 D1 (a) k+3 2k+7 k+4 3k+9 2k+6 (b) 1 2 3 4 5 11 12 13 14 15 10 (c) 6789 Figure 24-8. Type 6: Z-shape. (a) Cross section geometry. (b) Integration point numbering. (c) Example for k = 2. D3 D4 D1 (a) (0,0) (i,j) (0,k+3) [i×(k+3)+j]+1 (0,k+3) (k+3,k+3) 1 2 3 4 5 9 10 11 12 13 14 15 18 20 23 25 19 24 17 22 16 21 (b) (c) Figure 24-9. Type 7: Trapezoidal. (a) Cross section geometry. (b) Integration point numbering. (c) Example for k = 2. D1 j = k+3 (i,j) j = 0 i = 0 i = 4(k+3) [j×4(k+3)+i]+1 82 62 22 42 20 21 40 81 61 41 60 80 100 (a) (b) (c) Figure 24-10. Type 8: Circular. (a) Cross section geometry. (b) Integration point numbering. (c) Example for k = 2. D1 D2 j = k+3 (i,j) j = 0 i = 0 i = 4(k+3) [j×4(k+3)+i]+1 20 82 62 42 22 21 40 41 61 81 60 80 100 (a) (b) (c) Figure 24-11. Type 9: Tubular. (a) Cross section geometry. (b) Integration point numbering. (c) Example for k = 2. D6 D5 D3 D2 (a) 2k+3 D4 D1 4k+7 6k+9 2k+4 4k+6 15 16 17 18 19 20 21 8 9 10 1112 13 14 (b) (c) Figure 24-12. Type 10: I-Shape 2. (a) Cross section geometry. (b) Integration point numbering. (c) Example for k = 2. D2 D1 (a) (0,k+3) (k+3,k+3) [i×(k+3)+j]+1 (i,j) (0,0) (0,k+3) (b) 21 16 11 22 17 12 24 19 14 25 20 15 10 23 18 13 (c) Figure 24-13. Type 11: Solid Box. (a) Cross section geometry. (b) Integration point numbering. (c) Example for k = 2. D4 2k+5 4k+9 5k+9 5k+10 6k+10 7k+11 6k+11 8k+12 7k+12 17 18 19 20 21 22 D3 D1/2 D1/2 D2 (a) 2k+4 4k+8 (b) 25 24 23 28 26 27 10 11 12 13 14 15 16 (c) Figure 24-14. Type 12: Cross. (a) Cross section geometry. (b) Integration point numbering. (c) Example for k = 2. D2/2 D4 D2/2 2k+6 D3 4k+11 6k+13 2k+5 4k+10 19 20 2122 23 24 25 10 11 12 13 14 15 16 17 18 D1 (a) (b) (c) Figure 24-15. Type 13: H-Shape. (a) Cross section geometry. (b) Integration point numbering. (c) Example for k = 2. D3 + 4k+9 6k+12 1718 19 20 212223 24 D1 6k+13 8k+16 2526 2728 2930 3132 + + (b) (c) 10 11 12 13 14 15 16 D4 (a) D2 Figure 24-16. Type 14: T-Shape 2. (a) Cross section geometry. (b) Integration point numbering. (c) Example for k = 2. D1/2 D4 D2 (a) 2k+4 1 2 3 4 5 6 7 8 D1/2 D3 4k+9 6k+12 6k+11 8k+4 17 18 19 20 21 22 23 24 25 26 27 28 29 30 2k+5 4k+8 9 10 11 12 13 14 15 16 (b) (c) Figure 24-17. Type 15: I-Shape 3. (a) Cross section geometry. (b) Integration point numbering. (c) Example for k = 2. D3 D2 D1 D3 2k+7 3k+10 k+3 3k+9 4k+12 k+4 2k+6 11 12 13 14 15 16 17 18 19 20 10 (a) (b) (c) Figure 24-18. Type 16: Channel 2. (a) Cross section geometry. (b) Integration point numbering. (c) Example for k = 2. D1 D3 D1 D4 (a) 2k+4 4k+6 4k+5 D2 6k+7 2k+3 10 11 12 13 14 15 16 17 18 19 (b) (c) Figure 24-19. Type 17: Channel 3. (a) Cross section geometry. (b) Integration point numbering. (c) Example for k = 2. D2 D4 D1 (a) 4k+9 6k+11 6k+10 8k+12 17 18 19 20 21 22 23 24 25 26 27 28 D3 2k+5 2k+4 4k+8 1 2 3 4 5 6 7 8 9 10 11 12 13 14 15 16 (b) (c) Figure 24-20. Type 18: T-Shape 3. (a) Cross section geometry. (b) Integration point numbering. (c) Example for k = 2. D6 D2 D3 D4 D1 (a) D5 2k+7 k+3 3k+8 3k+7 k+4 4k+8 2k+6 11 12 13 14 15 16 10 (b) (c) Figure 24-21. Type 19: Box Shape 2. (a) Cross section geometry. (b) Integration point numbering. (c) Example for k = 2. D1 (0,0) (0,k+3) (i,j) (0,k+3) [i×(k+3)+j]+1 (k+3,k+3) (k+3) 2+ [i×(k+3)+j]+1 The bottom half is the reflection of the top-half with ids offset by (k+3)2 (b) D3 D2 (a) 1 2 3 4 5 9 10 11 12 13 14 15 18 20 23 25 19 24 17 22 16 21 46 47 49 50 48 41 42 43 44 45 36 37 38 39 40 31 32 33 34 35 26 27 28 29 30 (c) Figure 24-22. Type 20: Hexagon. (a) Cross section geometry. (b) Integration point numbering. (c) Example for k = 2. D1 D4 D2 D3 (a) D4 4k+9 2k+4 6k+12 + + 6k+11 + 8k+14 + (b) 17 18 19 20 21 22 23 9 10 1112 (c) 24 25 26 27 28 29 30 16 15 14 13 Figure 24-23. Type 21: Hat-Shape. (a) Cross section geometry. (b) Integration point numbering. (c) Example for k = 2. D2 D6 D4 D3 D1 (a) 4k+10 2k+5 6k+13 D6 + + 6k+12 D5 8k+16 + 8k+15 + 14k+22 (b) 18 19 20 21 22 23 24 10 1112 13 25 26 27 28 29 30 31 17 16 15 14 32 33 34 35 36 37 38 39 40 41 42 43 44 45 46 47 48 49 50 (c) Figure 24-24. Type 22: Hat-Shape 2. (a) Cross section geometry. (b) Integration point numbering. (c) Example for k = 2. *INTEGRATION Purpose: Define user defined through the thickness integration rules for the shell element. This option applies to three dimensional shell elements with three or four nodes (ELEMENT_SHELL types 1-11 and 16) and to the eight node thick shell (ELE- MENT_TSHELL). See *PART_COMPOSITE for a simpler alternative to *PART + *SEC- TION_SHELL + *INTEGRATION_SHELL. Card 1 1 2 3 4 5 6 7 8 Variable IRID NIP ESOP FAILOPT Type I I I I Define NIP cards below if ESOP = 0. Card Variable Type 1 S F 2 WF 3 PID F I 4 5 6 7 8 VARIABLE DESCRIPTION IRID NIP ESOP Integration rule ID (IRID refers to IRID on *SECTION_SHELL card). Number of integration points Equal spacing of integration points option: EQ.0: integration points are defined below, EQ.1: integration points are equally spaced through thickness such that the shell is subdivided into NIP layers of equal thickness. s = 1 Δti midsurface Figure 24-25. In the user defined shell integration rule the ordering of the integration points is arbitrary. s = -1 VARIABLE FAILOPT DESCRIPTION Treatment of failure when mixing different constitutive types, which do and do not include failure models, through the shell thickness. For example, consider the case where a linear viscoelastic material model, which does not have a failure option, is mixed with a composite model, which does have a failure option. Note: If the failure option includes failure based on the time step size of the element, element deletion will occur regardless of the value of FAILOPT. EQ.0: Element is deleted when the layers which include failure, fail. EQ.1: Element failure cannot occur since some layers do not have a failure option. S WF Coordinate of integration point in range -1 to 1. Weighting factor. This is typically the thickness associated with the integration point divided by actual shell thickness, i.e., the Δ𝑡𝑖 𝑡 as seen in weighting factor for the ith integration point = Figure 24-25. VARIABLE PID DESCRIPTION Optional part ID if different from the PID specified on the element card. The average mass density for the shell element is based on a weighted average of the density of each layer that is used through the thickness. When modifying the constitutive constants through the thickness, it is often necessary to defined unique part IDs without elements that are referenced only by the user integration rule. These additional part IDs only provide a density and constitutive constants with local material axes (if used) and orientation angles taken from the PID referenced on the element card. In defining a PID for an integration point, it is okay to reference a solid element PID. The material type through the thickness can vary. Interface definitions may be used to define surfaces, nodal lines, and nodal points for which the displacement and velocity time histories are saved at some user specified frequency. This data may then used in subsequent analyses as an interface ID in the *INTERFACE_LINKING_DISCRETE_NODE as master nodes, in *INTERFACE_LINK- ING_SEGMENT as master segments and in *INTERFACE_LINKING_EDGE as the master edge for a series of nodes. This capability is especially useful for studying the detailed response of a small member in a large structure. For the first analysis, the member of interest need only be discretized sufficiently that the displacements and velocities on its boundaries are reasonably accurate. After the first analysis is completed, the member can be finely discretized in the region bounded by the interfaces. Finally, the second analysis is performed to obtain highly detailed information in the local region of interest. When beginning the first analysis, specify a name for the interface segment file using the Z = parameter on the LS-DYNA execution line. When starting the second analysis, the name of the interface segment file created in the first run should be specified using the L = parameter on the LS-DYNA command line. Following the above procedure, multiple levels of sub-modeling are easily accommodated. The interface file may contain a multitude of interface definitions so that a single run of a full model can provide enough interface data for many component analyses. The interface feature represents a powerful extension of LS-DYNA’s analysis capabilities. The keyword cards for this purpose are: *INTERFACE_COMPENSATION_NEW *INTERFACE_COMPONENT_OPTION *INTERFACE_LINKING_DISCRETE_NODE_OPTION *INTERFACE_LINKING_EDGE *INTERFACE_LINKING_SEGMENT *INTERFACE_SPRINGBACK_OPTION1_OPTION2 Interface definitions may also be employed to define soil-structure interfaces in earthquake analysis involving non-linear soil-structure interaction where the structure may be non-linear but the soil outside the soil-structure interface is assumed to be linear. Free-field earthquake ground motions are required only at the soil-structure interface for such analysis. The keyword cards for this purpose are: *INTERFACE_SSI *INTERFACE_SSI_AUX *INTERFACE_SSI_STATIC *INTERFACE_BLANKSIZE_{OPTION} Available options include: DEVELOPMENT INITIAL_TRIM INITIAL_ADAPTIVE SCALE_FACTOR SYMMETRIC_PLANE Purpose: This keyword causes LS-DYNA to run a blank-size development calculation instead of a finite element calculation. The input for this feature consists of (1) the result of a completed metal forming simulation, (2) the corresponding initial blank, and (3) the desired result from the simulation in the form of a boundary curve or full mesh. From these inputs the *INTERFACE_BLANKSIZE method adjusts the initial blank so that the resulting formed piece more closely matches the target. The blank’s starting geometry may be systematically improved by iterating. A GUI for using this available in LS- SPACE Target curves (FILENAME1, target.xyz) Reference surface (FILENAME13, ref4.k) Final blank (FILENAME2, final.k) Initial blank (FILENAME3, initial.k) Modified initial blank boundary (trimcurves.ibo) Reference surface (FILENAME4, ref3.k) Figure 25-1. Trim curve development using a reference surface. See Example II. PrePost as of version 4.2 under APPLICATION → Metal Forming → Blank Size/Trim line. NOTE: When this card is present LS-DYNA does not proceed to the finite element simulation. This keyword requires one or all three keyword options, each corresponding to a different kind of forming operation: 1. DEVELOPMENT. This option takes as its target either a full mesh or a minimum boundary. It adjusts the blank so that he product more closely ap- proximates the target. The computed blank-boundary is written to a file called trimcurves.ibo, which contains a *DEFINE_CURVE_TRIM_3D keyword. 2. 3. INITIAL_TRIM. This option adjusts the blank so that trimming and mesh- refinement are mapped back onto the initial blank. INITIAL_ADAPTIVE. This option reads in (1) the input mesh for a flanging simulation as well as (2) the adapted mesh calculated during flanging simula- tion. It maps the refinement back to the initial blank. Card set for *INITIAL_BLANKSIZE_DEVELOPMENT. Development Parameter Card. Card 1 1 2 3 4 5 6 7 8 Variable IOPTION IADAPT MAXSIZE REFERENC SPACE MAXGAP ORIENT Type I Default -2 I 1 F I F F I 30.0 none 2.0 30.0 none Blanking OP10 Draw OP20 Trim OP30 Flanging Figure 25-2. A stamping process consists of draw, trim and flanging (Courtesy of Metal Forming Analysis Corporation). The labels OP10, OP20, and OP30 are used extensively in the ensuing discussion. Target Card. See “Target curves (target.xyz)” in Figure 25-1. Card 2 1 2 3 4 5 6 7 8 Variable Type Default FILENAME1 A80 none Final Blank Card. See “Final blank (final.k)” in Figure 25-1. Card 3 1 2 3 4 5 6 7 8 Variable Type Default FILENAME2 A80 none Initial Blank Card. See “Initial blank (initial.k)” in Figure 25-1. Card 4 1 2 3 4 5 6 7 8 Variable Type Default FILENAME3 A80 none Reference Surface Card. See “Reference surface (ref3.k)” in Figure 25-1 and Example II. Card 4 1 2 3 4 5 6 7 8 Variable Type Default FILENAME4 A80 none Reference Surface Card. See “Reference surface (ref4.k)” in Figure 25-1 and Example II. Card 4 1 2 3 4 5 6 7 8 Variable Type Default FILENAME13 A80 none Card set for *INTERFACE_BLANKSIZE_INITIAL_TRIM. Initial Flat Blank. FILENAME5 should specify the mesh of a blank that has been refined during a subsequent forming operation. FILENAME5 is usually set to the adapt.msh output. See “OP10 Initial Adapted blank mesh” in Figure 25-3. Card 1 1 2 3 4 5 6 7 8 Variable Type Default FILENAME5 A80 none Formed blank. FILENAME6 specifies a dynain file from a forming simulation. See “OP10 Final Blank” in Figure 25-3. Card 2 1 2 3 4 5 6 7 8 Variable Type Default FILENAME6 A80 none OP10 initial adapted blank mesh (.msh) OP10 final blank (adapted) OP20 final blank (adapted around hole) OP20 flat new (intermediate output) OP30 Target (nearly uniform tool mesh) OP30 flat new (more mesh around hole, intermediate output) OP30 initial blank (more mesh around hole, .msh file) OP30 initial blank (adapted) OP30 final blank (more mesh around hole) OP10 flat trim outline (output)) Figure 25-3. Inputs and outputs (Courtesy of Metal Forming Analysis Corp.). For exposition of labels OP10, OP20, and OP30 see Figure 25-2. Trimmed Formed Blank. A dynain file from a trimming simulation that started with the state given in FILENAME6. See “OP20 Final Blank” in Figure 25-3. Card 3 1 2 3 4 5 6 7 8 Variable Type Default FILENAME7 A80 none Trimmed Flat Blank (output). This field specifies the name for the file to which the trimmed flat blank is written. See “OP20 Flat New” in Figure 25-3. Card 4 1 2 3 4 5 6 7 8 Variable Type Default FILENAME8 A80 none Card set for *INTERFACE_BLANKSIZE_INITIAL_ADAPTIVE. Flat Blank. FILENAME9 specifies the mesh of a blank in a flat configuration serving as the basis for a two-step metal forming process. The second-stage simulation produces an adapt.msh file, from which the refinements are to be mapped onto the flat-blank of FILENAME9. See, for example, “OP20 Flat New” in Figure 25-3 where FILENAME9 points to result, FILENAME8, of an INITIAL_TRIM calculation. Card 1 1 2 3 4 5 6 7 8 Variable Type Default FILENAME9 A80 none Initial Blank. FILENAME10 is the result from the first stage of a two-step process. See, for example, “OP30 Initial Blank” in Figure 25-3 where FILENAME10 has been formed and trimmed and refined along the way. Card 2 1 2 3 4 5 6 7 8 Variable Type Default FILENAME10 A80 none Adapted Initial Blank. FILENAME11 contains a refined version of the mesh in FILENAME10. It is expect to name the adapt.msh file from some operation performed on the mesh of FILENAME10. See, for example, “OP30 Initial Blank (with more mesh)” in Figure 25-3, where the adapt.msh file comes from a flanging simulation. Card 3 1 2 3 4 5 6 7 8 Variable Type Default FILENAME11 A80 none Refined Flat Blank (output). This field specifies the name of the file to which the refined flat blank is written. The blank’s mesh is refined to exactly match the forming process. See, for example, “OP30 Flat New” in Figure 25-3. Card 4 1 2 3 4 5 6 7 8 Variable Type Default FILENAME12 A80 none Card set for *INTERFACE_BLANKSIZE_SCALE_FACTOR. Scale Factor Card. Define one card for each curve. Include as many cards in the following format as desired. This input ends at the next keyword (“*”) card. Card 1 1 Variable IDCRV Type Default I 1 2 SF F 0.0 3 4 5 6 7 8 OFFX OFFY OFFZ F 0 F 0 F 0 Card set for *INTERFACE_BLANKSIZE_SYMMETRIC_PLANE. Symmetric Plane Card. Card 1 Variable 1 X0 Type F 2 Y0 F 3 Z0 F 4 V1 F 5 V2 F 6 V3 F 7 8 Default 0.0 0.0 0.0 1.0 0.0 0.0 VARIABLE DESCRIPTION IOPTION Target curve definition input type: EQ.1: (entire) blank mesh in keyword format. EQ.2: consecutive position coordinates of blank boundary loop curve in XYZ format, defined by *DEFINE_TAR- GET_BOUNDARY. The blank mesh’s normal vector and the closed boundary curve are consistently orient- ed according to the right-hand rule, see Figure 25-4. Note the target boundary curves must have enough points for a successful prediction of the initial blank size. Starting in Revision 100589, curve direction is de- sensitized, meaning both IOPTION = 2 and IOP- TION = -2 will give the same results. EQ.-2: consecutive position coordinates of blank boundary loop in XYZ format, defined by *DEFINE_TARGET_- BOUNDARY. The blank mesh’s normal vector and the closed boundary curve are consistently oriented ac- cording to the left-hand rule, see Figure 25-4. Note the target boundary curves must have enough points for a successful prediction of the initial blank size. Starting in Revision 100589, curve direction is desensitized, meaning both IOPTION = 2 and IOPTION = -2 will give the same results. In LS-PrePost 4.0, menu option GeoTol → ID Measure can be used to show the flow direction of a boundary curve. Curve → Rever(se) can be used to reverse the curve direction. mesh normal direction mesh normal direction IOPTION=2 IOPTION=-2 Figure 25-4. Differences between IOPTION 2 and -2. Note Starting in Revision 100589, curve direction is desensitized, meaning both IOPTION = 2 and IOPTION = -2 will give the same results. VARIABLE IADAPT DESCRIPTION Adaptive mesh control flag. If IADAPT = 1, number of elements between initial (FILENAME3) and simulated blank (FILE- NAME2) meshes can be different, so it is not necessary to use the sheet blank from the file “adapt.msh” (created by setting IOFLAG = 1 in *CONTROL_ADAPTIVE) for the initial blank mesh. MAXSIZE The maximum change in initial blank size in each iteration. It is used to limit the blank size change in each iteration during mapping to avoid convergence problems when the initial blank is curved. REFERENC Flag to indicate trim curve projection to a reference surface (mesh), see Figure 25-1: EQ.0: no projection. EQ.1: the trim curves will be projected to the reference surface. In addition, the mesh file for the reference surface is given in FILENAME4. VARIABLE SPACE DESCRIPTION Point spacing distance on the reference surface for the projected curve, see Figure 25-1. If the gap between two neighboring points in the modified trimming curve is larger than this value, extra nodes will be added in the final blank and projected to the reference surface. Smaller value should be used for large reference surface curvature. MAXGAP When REFERENC is set to “1”, the nodes from the final blank will be projected to the reference surface. However, if the distance between the nodes and the surface is larger than MAXGAP, the nodes will not be projected. ORIENT A flag to control iterative optimization efficiency or to include a reference surface file for the final formed blank. EQ.1: activates a new algorithm to potentially reduce the number of iterations during iterative blank size optimi- zation loop, to be used in conjunction with the option SCALE_FACTOR (0.75~0.9). EQ.2: to (in include a reference surface FILENAME13 keyword mesh format) for the simulated (formed) blank. This is useful when formed blank is smaller than intended and extended surface are not flat. See Remarks and Figure 25-1. Target input file name. When a blank mesh is used (IOP- TION = 1), the keyword file must contain *NODE and *ELE- MENT_SHELL keywords. When using the blank boundary curve for target (|IOPTION| = 2), the file must consist of *DE- FINE_TARGET_BOUNDARY. See the Target Boundaries (and IGES) in the remarks section. Simulated (formed or flanged) sheet blank mesh in keyword format. This mesh can be obtained from the final state of any downstream process simulation. Initial sheet blank mesh in keyword format. This can be the first state mesh from any process simulation prior to FILENAME2 simulation. Set IADAPT = 1 if adaptive refinement is used in any simulation. FILENAME1 FILENAME2 FILENAME3 VARIABLE FILENAME4 FILENAME5 FILENAME6 FILENAME7 DESCRIPTION Reference surface onto which adjustments to the blank’s trim curves in its initial state are projected (ref3.k in Figure 25-1). This surface is typically a curved extension of the initial blank and must be defined as mesh in keyword format. This file name must be defined when REFERENC is set to 1. Also see extended reference surface for the final state (formed state) - FILE- NAME13. Initial blank in its flat configuration with adapted mesh in keyword format. FILENAME5 usually points to an adapt.msh file. For example see OP10 in Figures 25-2, 25-22 and 25-3, in which FILENAME5 is the adapt.msh from a draw-forming calculation. Final formed blank in keyword format. This is usually the dynain file corresponding to the adapt.msh file mentioned above for FILENAME5, see Figures 25-2, 25-22 and 25-3. A trimmed blank in keyword format. This file should be derived from FILENAME6 as the dynain file from a trimming simulation. See OP20 in Figures 25-2, 25-22 and 25-3. FILENAME8 This field specifies the name for the file in which the trimmed flat blank is to be written. See OP20 in Figures 25-2, 25-22 and 25-3. FILENAME9 FILENAME9 should point to the blank defined by FILENAME8, as in Figures 25-2, 25-22 and 25-3. FILENAME10 FILENAME11 Initial-stage result file name. This may be extracted from d3plot files using LS-PrePost or it may be generated by LS-DYNA as a dynain file. See, for example, “OP30 Initial Blank” in Figure 25-3 where FILENAME10 has been formed, trimmed and refined along the way. To obtain from d3plot file the necessary mesh in keyword format using LS-PrePost4.0 select POST → OUTPUT → Dynain ASCII and check the box for “Exclude strain and stress”. FILENAME11 contains a refined version of the mesh in FILENAME10. FILENAME11 can be obtained from adapt.msh file from the same operation performed on the mesh of FILENAME10. See, for example, “OP30 Initial Blank (with more mesh)” in Figure 25-3, where the adapt.msh file comes from a flanging calculation. VARIABLE FILENAME12 FILENAME13 IDCRV SF OFFX, OFFY, OFFZ DESCRIPTION This field specifies the name of the file to which the refined flat blank is written. The blank’s mesh is refined to exactly match the forming process. See, for example, “OP30 Flat New” in Figure 25-3. Reference surface onto which adjustments to the blank’s trim curves in its final state are projected (ref4.k in Figure 25-1). This surface is typically a curved extension of the formed blank and must be defined as mesh in keyword format. This file name must be defined when ORIENT is set to 2. Curve ID in the order of appearance as in FILENAME1 in the target card, as defined by *DEFINE_TARGET_BOUNDARY. Scale factor for the IDCRV defined above. It defines a fraction of the changes required for the predicted initial blank shape. For example, if SF is set to “0.0” the corresponding IDCRV will be excluded from the calculation (although the original initial curve still will be output); on the other hand, if SF is set to “1.0”, full change will be applied to obtain the modified initial blank that reflects the forming process. A SF of 0.5 will apply 50% of the changes required to map the initial blank. This feature is especially important for inner holes that are small and hole boundary expansions are large, so the predicted initial hole can avoid “crisscross” situation. An example is provided in Scale Factor and Symmetric Plane. Translational move of the target curve. This is useful when multiple target curves (e.g. holes) and formed curves are far away from each other. Input values of OFFX, OFFY and OFFZ helps establish one-to-one correspondence between each target curve and formed curve. OFFX.EQ.-10000.0: offset values are automatically calculated. X0, Y0, Z0 V1, V2, V3 𝑥, 𝑦, 𝑧 coordinates of a point on the symmetric plane. See example in Scale Factor and Symmetric Plane. Vector components of the symmetric plane’s normal. See example in Scale Factor and Symmetric Plane. Compulational Cost Accuracy Information Required Physical Process Blanksize Full simulation Exact Full Simulation Any Unflanging Fast Approximate Process Geometry Inverse Flanging Onestep Fast Approximate None (Path independent) Any Table 25-1. Comparison of inverse methods. Inverse Methods for Optimizing Blank Size and Trim Lines: Finding the minimal practicable blank size and developing an optimal set of trim lines is an integral part of the die engineering process. This card, *INTERFACE_BLANK- SIZE, is one of several features that have been developed to solve the inverse problem: that is to calculate an initial blank or blank boundary that will yield a desired product based mostly on the target geometry of that final product. 1. The One-Step Method. The *CONTROL_FORMING_ONESTEP card is suitable for early blank-size estimates. It invokes the total-strain theory of plas- ticity thereby bypassing the, as of yet, undetermined specific details of the forming process. 2. Unflanging. Once product design and process plan are complete, die development begins with addendum and binder creation, followed by second- ary tooling development. In this stage, *CONTROL_FORMING_UNFLANG- ING can be used to develop trim lines for the secondary tooling; final (or intermediate) desired flange shapes are unfolded onto the addendum or binder to obtain the corresponding flange shapes in its initial shape. It also imple- ments failure criteria to arrive at suggested final flange curves, with strains and thickness output on the unfolded flanges. 3. Interface Blanksize. This card, *INTERFACE_BLANKSIZE, can be used to accurately determine the optimal initial blank. To do so it requires on initial configuration, the corresponding simulated configuration, and a desired target configuration. This method takes into account the entire metal-forming pro- cess. a) One application of this keyword is to map trim curves between dies to calculate the trim curves needed for all trim dies. An example of the ap- plication can be found in Figures 25-18 through 25-21. Draw(flanging) simulation Initial blank Final blank Target blank/boundary Reference surface *INTERFACE_BLANKSIZE _[OPTION] Final blank size within tolerance of the target blank? Yes Done DOS or linux commands No Figure 25-5. An iterative blank size development process. b) The keyword can also be used to determine the precise minimal initial blank needed for a draw panel whose blank edge must be at specified dis- tances from the edge of the draw beads. Iterative Workflow: The “interface blanksize” command produces an adjusted initial blank. It is not to be expected that the adjustment will be exact. However, this initial blank shape can be run through a second simulation to see if the final shape is close enough to the target blank. If it is not close enough, then the results from the second simulation can be used to repeat the process. Iterations can proceed until the final shape is within the range of the target shape. This iterative blank size development process is schematically presented in Figure 25-5 and exemplified in Figures 25-8 through 25-17. Target Boundaries (and IGES): When IOPTION = 2, or -2, a file with the keyword *DEFINE_TARGET_BOUNDARY must be present. This keyword can now be created from an IGES file using LS- PrePost4.1 (or 4.2). To convert from IGES curves to keyword *DEFINE_TARGET_- BOUNDARY in LS-PrePost4.1, use menu option Curve → Convert→ Method (To Keyword) → Select *DEFINE_TARGET_BOUNDARY; pick the curves then hit “To Key”; write out the keyword file using File → Save as → Save Keyword As, and select “Output Version” as “V971_R7”. In LS-PrePost 4.2, a GUI interface was developed located at Applica- tion/Metal Forming/Blanksize Trimline so users can import the target curve directly in IGES format, the initial and final blank mesh and then write out a complete LS-DYNA input deck. In addition, the target curves should be projected onto the final blank mesh if they do not exactly lie on the mesh surface. This can be done with LS-PrePost4.1 via the menu option GeoTol → Project → Project, select Closest Projection, select Project to Elements, then define the destination mesh and source curves, and hit Apply. 3-D projection in LS- PrePost4.2 can be critical in obtaining a perfectly smooth predicted initial boundary curve trimcurves.ibo after the LS-DYNA run. Note the projected target curves should be used to import into the GUI. Computed Initial Blank Boundaries (and IGES): Computed boundary curves are written with *DEFINE_CURVE_TRIM_3D keyword into a file called trimcurves.ibo. The format of this file follows the keyword’s specification. LS-PrePost4.0 can convert the computed curve to IGES. See Figure 25-10. After hitting Apply, the curves will show up in the graphics window, and File → Save as → Save Geom as can be used to write the curves out in IGES format. In the LS-PrePost4.2 GUI, under Results, trimcurves.ibo can be directly imported into the graphics window for viewing and to save in either STEP or IGES format. To convert IGES to the *DEFINE_CURVE_TRIM_3D keyword format import the IGES file into LS-PrePost4.0, and follow the procedures shown in Figure 25-11. After finishing step 2, “curves have been converted to keyword format” will be reported in the command prompt. Then use File → Save → Save keyword to write out the keyword file. Support for Multi-Stage Processes with the Development Option: Original Implementation. Prior to Revision 88708 the development option required that the final blank (FILENAME2) differ from the initial blank (FILENAME3) by no more than a deformation and mesh refinement. In practice, this means that the two meshes must come from the same process simulation. For example, in a draw, trim and flanging process, the trimmed panel mesh is used for flanging simulation. Therefore, with the original implementation, LS-DYNA required that the initial blank state (FILENAME3) be trimmed when the final blank state (FILENAME2) is flanged on trimmed panel. Failure to observe this limitation may result in error termination. Output: predicted initial blank outline (station 1) Input: initial blank shape (station 1) Input: target part boundary outline (station 2) Input: simulated blank final shape (station 2) Figure 25-6. Blank size development in a progressive die with IADAPT = 1 in Example I Enhanced Implementation. A more recent improvement to the blank size development (Revision 88708) removes the requirement that initial (FILENAME3) and final (FILENAME2) blanks must be from the same process simulations. The initial and final blank states may differ by a trimming process. This allows trimming and other process such as flanging to occur between the initial and final blanks, without the need of invoking the INITIAL_TRIM and INITIAL_ADAPTIVE options. For example, the initial blank can be the blank mesh from “Blanking” in Figure 25-2, and the final blank can be the blank mesh from “Flanging,” which is also in Figure 25-2. Scale Factor and Symmetric Plane: An example of using various scale factors ranging from 0.0 to 1.0 on a model involving an initial hole shape is shown in Figure 25-25. The target curve is given in targetline.k. All nodes along the symmetric plane are constrained by the SYMMETRIC_PLANE option. The symmetric plane is defined going through point coordinates (-76, 2.63844, 0.38) with plane normal vector of (1.0, 0.0, 0.0). A complete input is provided below: *KEYWORD *INTERFACE_BLANKSIZE_DEVELOPMENT $ IOPTION IADAPT -2 1 $ target boundary curves targetline.k $ final formed mesh final.k $ initial mesh initial.k *INTERFACE_BLANKSIZE_SCALE_FACTOR $ IDCRV SF 1 0.2 *INTERFACE_BLANKSIZE_SYMMETRIC_PLANE $ X0 Y0 Z0 V1 V2 V3 -76 2.63844 0.38 1.0 0.0 0.0 *END If taregetline.k consists of multiple curves, the following format can be used: *INTERFACE_BLANKSIZE_SCALE_FACTOR $ IDCRV SF 1 0.2 2 0.8 3 1.0 ⋮ ⋮ Example I: Simple Example of the Development Option Given the initial and final blank configuration and a target, this option calculates a new initial blank outline, corresponding to the target final blank boundary. In this example note that IADAPT = 1, meaning initial and final blank meshes may differ by an adaptively operation. The input and output files are detailed below, and output results are shown in Figure 25-6. *KEYWORD *INTERFACE_BLANKSIZE_DEVELOPMENT $ IOPTION IADAPT 2 1 $ input file for target mesh, or target position coordinates targetpoints.k $ input file for formed mesh final.k $ input file for initial blank mesh initial.k *END The file, targetpoints.k, is partially shown below was generated from IGES using LS- PrePost 4.1. *KEYWORD *DEFINE_TARGET_BOUNDARY -1.83355e+02 -5.94068e+02 -1.58639e+02 -1.80736e+02 -5.94071e+02 -1.58196e+02 -1.78126e+02 -5.94098e+02 -1.57813e+02 -1.75546e+02 -5.94096e+02 -1.57433e+02 -1.72888e+02 -5.94117e+02 -1.57026e+02 ⋮ ⋮ ⋮ -1.83355e+02 -5.94068e+02 -1.58639e+02 *END The output is the modified initial blank outline in the file trimcurves.ibo. Example II: The Reference Surface feature for the Development Option For an initial blank that is not flat, the fields REFERENC and FILENAME4 can be used to define a surface onto which changes in the boundary are needed. This is important when the adjusted boundary is not a simple tangential extension of the initial blank. In a keyword example below, REFERENC is set to “1” and the reference file for the extended initial shape is given as ref3.k. The maximum change between the initial and final blank size is set to be 20.0 mm per iteration. Point spacing distance (SPACE) of calculated trim curve on the reference surface is set at 2.0 mm. Note that the inner holes and outer boundary curves are defined in “target.xyz”. The holes do not necessarily need to exist in the initial or final blank mesh. Also, since ORIENT is set to “2”, a reference surface mesh file (ref4.k) is provided for the final (formed) state. The input details and output results are shown in Figure 25-1. *KEYWORD *INTERFACE_BLANKSIZE_DEVELOPMENT $ 1 2 3 4 5 6 7 8 $ IOPTION IADAPT MAXSIZE REFERENCE SPACE ORIENT -2 1 20.000 1 2.0 2 $ input file for target mesh: target.xyz $ input file for formed mesh: final.k $ input file for initial blank mesh: initial.k $ reference file for extended initial shape: ref3.k $ reference file for extended final shape: Ref4.k *END Blank edge 10mm outside of last draw bead bend Cross Member in Air Draw Target Blank Edges 10 mm Outside of Beads Figure 25-7. NUMISHEET 2005 cross member in Exmaple III. Example III: Development Feature Applied to a Draw Die with Physical Bead In this example, which was created from NUMISHEET 2005, the DEVELOPMENT option has been used to design a blank such that, when formed, the edge is a specified distance outside of the last bend of a draw bead. In Figure 25-7, the tooling and blank set up is shown to the left. The right side of the figure shows the target blank, whose left and right edges everywhere are made 10mm outside of the last bending radius of the draw beads. This setup is prototypical of one method to ensure a very stable and high-quality stamping process. The first step towards setting up this analysis was to use *CONTROL_FORMING_ON- ESTEP to unfold the target blank and thereby obtain an initial guess of a flat blank, as shown to the left if Figure 25-12. The flat blank is then formed as one would usually do in a regular forming simulation, shown on the right side of the figure. The formed blank (Iteration 0) turns out to be larger than the target. Next, the DEVELOPMENT is applied to generate a new and better initial blank that will lead to the target blank. The flat blank is used as input for the “initial blank mesh”, the formed blank is used as input for the “simulated mesh”, and the target blank mesh, or boundary points is used to define the target. In Figure 25-13 (left) the improved initial blank, called the first compensated blank, is superimposed onto the original one-step unfolded result. The one-step unfolded result is somewhat larger than the developed blank. When formed the improved blank (Iteration 1) nearly overlaps the target blank, shown in Figure 25-13 (right). If the final formed blank still deviates from the target, another iteration would ensue, until satisfactory results are obtained. Gravity loaded Binder surface Figure 25-8. NUMISHEET 2008 B-pillar; Gravity loaded blank. Lower punch Example IV: Iterating with the Development Option Because the NUMISHEET 2008 B-pillar model involves neither trimming nor flanging, it exmplifies the DEVELOPMENT option in its most direct use case. This model, illustrated in Figure 25-8, simulates a draw-die’s action on a gravity-stressed flat blank. The B-pillar undergoes a stamping process including gravity, binder closing, and being drawn. In this example the DEVELOPMENT option is used to calculate the geometry for an initial blank that will exactly satisfy the design specification for a final formed panel. To highlight the efficiency of this feature, we start with an initial blank whose formed product deviates from the specification by a wide margin and then iterate using the DEVELOPMENT feature. The target and the optimal initial blank are shown in Figure 25-14. The intial guess is intentionally deviated from the optimal initial blank as shown in the left panel of Figure 25-15; while the formed blank is compared with the target in the right panel. In the first iteration a new initial blank is computed, and illustrated in the left panel of Figure 25-16 bearing the label, 1st compensated blank. The simulation is repeated using the first compensated blank, and in the right panel the result is compared to the target. The formed blank is narrower in the notched areas as compared with the target. The second iterate is shown in the left panel of Figure 25-17 bearing the label, 2nd compensated blank. Again, the simulation is repeated, but this time using the second compenated blank, and the result is compared to the target in the right panel of Figure 25-17. The resulting product is a good match to the target. Because of the initial blank was intentionally deviated from its ideal shape by a large margin, this example requires two iterations to converge. Generally this processed is bootstrapped with the *CONTROL_FORMING_ONESTEP card, which calculates an initial guess by approximately unfolding the target shape. Forming Trimming Blanking (OP10 initial blank) OP10 OP20 Forming Bending Flanging OP30 OP40 OP50 Courtesy of T&D Design, LLC, U.S.A Flanging Figure 25-9. Enhanced DEVELOPMENT feature on a progressive die. Even though trimming occurs at OP20 the algorithm requires as input only OP10, OP50, and a target geometry. Example V: Development Feature Applied to Flanging Process In this example, which is schematically illustrated in Figure 25-18, the NUMISHEET 2002 fender outer is flanged along the hood line. The development feature adjusts the initial blank’s boundary so that the formed piece matches the specified target flanged shape as shown in Figure 25-19. For demonstration purposes, the trimmed blank shape is intentionally deviated from the optimal configuration by a large amount. This error is indicated in Figure 25-20 by the label initial guess trim curves. In Figure 25-20 The flanged product is shown to deviate substantial from the flanged target along the boundary. As shown in Figure 25-21 after one iteration the correct initial blank boundary is obtained. Alternatively, *CONTROL_FORMING_UNFLANGING can be used to unfold the flanged target onto the addendum to obtain the initial blank size, or a starting guess for this process. Example VI: Enhanced-Development Feature Applied to Progressive Die Process In the example of Figure 25-9, courtesy of T&D Design, LLC, U.S.A, the blank-shape for a five stage progressive die process is calculated. Because this process involves a trimming step, the development capability prior to Revission 88708 does not support this example. In this example, an initial blank at OP10, undergoes trimming, reforming, bending and flanging to arrive at the blank in OP50. In figure 25-23 the computed product is compared with the specified target. A blank size development calculation produces the modified OP10 initial blank outline. The updated blank is used in a verification simulation. As seen in Figure 25-24 the blank size development feature produces a good result. Trim lines are not optimized by the development feature, so trimming should only occur along the boundary of the target blank. The modified OP10 blank requires some refitting in the trimmed area. Revision information: This feature is available in both SMP and MPP, in double precision only. Note a GUI for using this feature is now available in LS-PrePost as of version 4.2. It can be accessed under APPLICATION → Metal Forming → Blank Size/Trim line Dev. Starting revision information for each feature is listed as follows: 1. DEVELOPMENT option: Revision 74605. 2. 3. INITIAL_TRIM and INITIAL_ADAPTIVE: Revision 75023. IADAPT: Revision 75827. 4. Command line option “JOBID=…”: Revision 82861. 5. MAXSIZE: Revision 85633. 6. SPACE: Revision 85755. 7. MAXGAP: Revision 85792. 8. Reference surface (parameter REFERENC): Revision 86086. 9. Removal of the restriction requiring the initial (FILENAME3) and the final (FILENAME2) blanks must be from the same process simulation: Revision 88708. 10. Improve smoothness of the output trim curve trimcurves.ibo in case the given meshes have warpage caused by wrinkles during forming: Revision 96164. 11. Symmetric plane: Revision 97443. 12. Scale factor: Revision 98122. 13. ORIENT = 1: Revision 100453. 14. ORIENT = 2: Revision: 104168. 15. Curve direction is desensitized, meaning both IOPTION = 2 and IOPTION = -2 will give the same results: Revision 100589. 16. OFFX, OFFY, OFFZ: Revision 100660. 17. Automatically calculate offset values (OFFX.EQ.-10000.0): Revision 102609. SelPart RefGeo Keyword Manage Keyword Edit Keyword Search Keyword Curve CreEnt Surf PartID Solid Display GeoTol RefChk Mesh Renum Model Section EleTol MSelect Post Subsys MFPre Groups MFPost Views Favor1 PtColor Edit: DEFINE_CURVE_TRIM_3D Edit Model All RefBy 3 (right click) Name Count DEFINE 1 CURVE_TRIM_3D 1 KEYWORD 1 KEYWORD 1 TITLE 1 Delete all Delete by ids Transfer to Transfer to Curve Material arrange GroupBy Sort List Model Type All Load From MatDB Model Check ExpandAll Keyword Del CollapseAll Done Transfer to Curve DEFINE_CURVE_TRIM_3D(1) From 1 To All None Reverse Apply Done Figure 25-10. Converting trimcurves.ibo to IGES format in LSPP4.0. 1 (right click) Assembly 1 Shape Group BSpline Edge 1: Curve Geom Parts (un)Blank Reverse Blank Delete Rename Color Transparent Locate Locate by ID... Statistical To 2.x To Keyword Curve Trim 3D Sort by ID Sort by Type Figure 25-11. Converting IGES file to *DEFINE_CURVE_TRIM_3D. One-step unfold result with *CONTROL_FORMING_ONESTEP Iteration 0: formed from one-step unfolded blank Drawn blank 10mm outside of draw beads - Target Target Figure 25-12. Initial blank calculation and baseline formed blank. 1st compensated blank using this keyword Iteration 1: Formed from 1st compensated blank Original one-step unfold result Target Figure 25-13. The first compensated blank and the final confirmation run. Target blank Target blank formed Figure 25-14. Assumed target blanks. Target blank Initial guess Formed from initial guess Target blank formed Figure 25-15. Iteration 0 results comparison with target. Target blank 1st compensated blank Formed from 1st compensated blank Target blank formed Figure 25-16. Iteration 1 results. Target blank 2nd compensated blank Formed from 2nd compensated blank Target blank formed Figure 25-17. Iteration 2 results. Lower post Flanging steel move Figure 25-18. The flanging process on NUMISHEET 2002 fender outer. Drawn and trimmed Pressure pad *INTERFACE_BLANKSIZE Addendum / binder surface where trim lines to be developed Target part (flanged part) Drawn panel to be trimmed for flanging Figure 25-19. Multiple section view showing the target part and addendum surfaces. Flanged shape based on initial guess trim curves, deviates from flanged target Initial guess trim curves intentionally off by a large margin Flanged target Figure 25-20. Initial trim curves intentionally made to be off by a large margin. Compensated trim curves Initial guess Compensated flanged part overlaps flanged target Figure 25-21. Compensated trim curves overlap with the target curves. OP10 final blank OP20 file name for calculated initial flat blank OP30 adapted initial blank mesh OP30 file name for calculated initial flat blank OP30 final blank OP10 initial adapted flat blank OP20 trimmed blank OP30 initial mesh (from OP30 d3plots of first state with adaptive constraints) *KEYWORD *INTERFACE_BLANKSIZE_INITIAL_TRIM case10.adapt.msh case10.dynain case20.dynain op20_flat_new *INTERFACE_BLANKSIZE_INITIAL_ADAPTIVE op20_flat_new case30start.k case30.adapt.msh op30_flat_new *INTERFACE_BLANKSIZE_DEVELOPMENT $ IOPTION 1 target.k case30.dynain op30_flat_new *END OP30 target OP30 initial flat blank User inputs LS-DYNA intermediate output files LS-DYNA simulation output: new trim line OP10 (file "trimcurves.ibo") Figure 25-22. File structures for a multi-process blank development. Input #3: OP10 initial blank Input #2: OP50 formed blank Output: modified OP10 initial blank outline Blanking Courtesy of T&D Design, LLC, U.S.A Input #1: OP50 target boundary OP50 Figure 25-23. Inputs and output for the enhanced DEVELOPMENT feature. OP50 formed blank outline Input #1: OP50 target boundary OP50 formed blank outline coincides with the target boundary Final OP50 formed blank is off target in areas indicated Courtesy of T&D Design, LLC, U.S.A Final OP50 formed blank meets target requirement with OP10 modified blank outline Figure 25-24. Verification simulation on a progressive die process. Initial blank (input) Final blank (input) Option SYMMETIC _PLANE applied on nodes along the symmetric plane (input) Output for scale factor: 1.0, or, without using option SCALE_FACTOR Output for scale Factor: 0.2 Final hole boundary (input) Output for scale factor: 0.0, or, original initial hole boundary. Target hole boundary (input) Figure 25-25. Options SCALE_FACTOR and SYMMETRIC_PLANE. *INTERFACE_COMPENSATION_NEW_{OPTION} Available options include: <BLANK> ACCELERATOR MULTI_STEPS LOCAL_SMOOTH PART_CHANGE REFINE_RIGID Purpose: This card encompasses several methods for spring back compensation in stamping tools. The applications for this card include: (1) calculating the deviation of the stamped part from its intended design, and to automatically compensate the tool to minimize the deviation; (2) to map the existing trim curve to the modified tool; and (3) to automatically detect undercut. This keyword employs a nonlinear iterative method. Usually, it takes between 2 and 4 iterations to converge within tolerances. Additionally, this method provides a scale factor, which allows the user to decide the ratio of shape deviation the part is compensated. Options The ACCELERATOR option speeds up the convergence rate in reducing the part deviation to design tolerance thus reducing the number of iterations. This option also allows for a much simpler user interface. The MULTI_STEPS option allows for tooling compensation of the next die process, based on target blank shape, compensated blank shape for the next step, and current tools. This feature is useful in line die process/tooling compensation. The LOCAL_SMOOTH option features smoothing of a tool’s local area mesh, which could become distorted because of either bad or coarse mesh of the original tool surface, or in areas where tooling pairs (for example, flanging post and flanging steel) do not maintain a constant gap, or after a few compensation iterations. The PART_CHANGE option allows for updating of the final compensated tool using the changed part or formed blank shape, thus eliminating the need for going through a new compensation iteration loop. This option is used together with *INCLUDE_COM- PENSATION_UPDATED_BLANK_SHAPE, and *INCLUDE_COMPENSATION_UP- DATED_RIGID_TOOL. The REFINE_RIGID option refines the rigid tool mesh based on user-provided trim curves. It also realigns the mesh so no elements cross the trim curves. This feature only needs to be done once before the iterative springback compensation begins. The modified rigid too mesh will greatly improve the convergence in the iterative process. Known Limitation The current methods sometimes fail to eliminate undercut. All required input files must be included by using various options in the keyword: *IN- CLUDE_COMPENSATION_{OPTION}. The option LOCAL_SMOOTH also needs to use a keyword *SET_NODE_LIST_SMOOTH. Card 1 for <BLANK>, MULTI-STEPS, and LOCAL_SMOOTH options. Card 1 1 Variable METHOD Type Default I 6 2 SL F 3 SF F 5.0 0.75 4 5 6 7 8 ELREF PSIDM UNDCT ANGLE NLINEAR I 1 F F F none none 0.0 I 1 Card 1 for keyword ACCELERATOR option. Card 1 1 2 3 4 5 6 7 8 Variable ISTEPS TOLX TOLY TOLZ OPTION Type Default I 0 F F F 0.5 0.5 0.5 I Card 1 for keyword option PART_CHANGE: Card 1 1 2 3 4 5 6 7 8 Variable MAXGAP Type F Default none Card 1 for keyword option REFINE_RIGID: Card 1 1 2 3 4 5 6 7 8 Variable Type Default FILENAME1 A80 none Card 2 for keyword option REFINE_RIGID: Card 1 1 2 3 4 5 6 7 8 Variable Type Default VARIABLE METHOD SL FILENAME2 A80 none DESCRIPTION There are several extrapolation methods for the addendum and binder outside of trim lines, see Remarks. The smooth level parameter controls the smoothness of the modified surfaces. A large value makes the surface smoother. Typically the value ranges from 5 to 10. If spring back is large, the transition region is expected to be large. However, by using a smaller value of SL, the region of transition can be reduced. VARIABLE DESCRIPTION SF Shape compensation scale factor. The value scales the spring back amount of the blank and the scaled amount is used to compensate the tooling. GT.0: compensate in the opposite direction of the spring back; LT.0: compensate in the punch moving direction (for undercut). This scale factor scales how much of the shape deviation is compensated. For example, if 10 mm of spring back is predicted, and the scale factor is chosen as 0.75, then the compensation in the opposite direction will only be 7.5 mm. Experience shows that the best scale factor for reaching a converged solution (within part tolerance) is case dependent. In some cases, a scale factor range of 0.5 to 0.75 is best; while in others, larger values are indicated. Sometimes, the best value can be larger than 1.1. Note that within an automatic compensation loop, this factor does not need to be varied. Since it is impossible to choose the best value for each application up front 0.75 is recommended for the first attempt. If the spring back cannot be effectively compensated and the calculation diverges, the factor can be moved upward or downward to obtain a converged solution, or more iterations must be used with the initial trial value to compensate the remaining shape deviation. For channel shaped parts that have a twisting mode of spring back, the scale factor is more important. It was found that a small change of the tool shape might change the twisting mode. If this occurs, using a small value (<0.5) is suggested. ELREF Element refinement option: EQ.1: special element refinement is used with the tool elements (default); EQ.2: special element refinement is turned off. VARIABLE PSIDM DESCRIPTION Define the part set ID for master parts. It is important to properly choose the parts for the master side. Usually, only one side (master side) of the tool will be chosen as the master side, and the modifications made to the other side (slave side) depends solely on the changes in the master. This allows the two sides to be coupled and a constant (tool) gap between the two sides is maintained. If both sides are chosen to be master, the gap between the two sides might change and become inhomogene- ous. The choice of master side will have an effect on the final result for method 7 when applied to three-piece draw models. At this time, when the punch and binder are chosen as the master side, the binder region will not be changed. Otherwise, when the die is chosen as master side the binder will be changed, since the changes extend to the edges of the master tool. UNDCT Tool undercut treatment option: EQ.0: no check (default); EQ.1: check and fix undercut. ANGLE An angle defining the undercut. NLINEAR Activate nonlinear extrapolation. ISTEPS Steps in accelerated compensation procedure, see Remarks. TOLX TOLY TOLZ Part deviation tolerance between current blank and target blank shape in global 𝑥-direction. Part deviation tolerance between current blank and target blank shape in global 𝑦-direction. Part deviation tolerance between current blank and target blank shape in global 𝑧-direction. OPTION Compensation acceleration method. Currently available only for method 1. MAXGAP Maximum gap between the original part and changed part. VARIABLE FILENAME1 FILENAME2 DESCRIPTION Rigid tool mesh file in keyword format. This should be the tooling mesh used in the forming or flanging simulation, before any compensation is done. The refined rigid tool mesh will be in the file rigid_refined.tmp. See Option REFINE_RIGID: rigid tool mesh refinement for a better convergence. Trim curves in keyword format *DEFINE_CURVE_TRIM_3D. The curves will be used to refine and realign the FILENAME1 to improve the convergence in the iterative compensation process. The refined rigid tool mesh will be in the file rigid_refined.tmp. See Option REFINE_RIGID: rigid tool mesh refinement for a better convergence. Compensation Methods Overview: After trimming, only a limited part of the tool has direct relationship with the spring back of the blank part. Modifications of the rigid tool outside the trimmed region involves extrapolation. Unfortunately, extrapolating is unstable and tends to generate non-smooth surfaces. To resolve this problem, seven smoothing algorithms are implemented. The most frequently used methods are methods 7, 8 and -8, while the others are used only occasionally. Method 7 If the punch is chosen as the master side, the binder will not be changed. Aside from the region inside the punch opening the rest of the model is untouched. Smoothing has little effect on method 7. The smoothness of the modified tool depends on the magnitude of the spring back and the size of the addendum region. This method is nonlinearly and, therefore, necessitates an iterative solve. Advantages: The binder will not be changed. Disadvantages: The change will be limited inside the addendum region, and the modified surface may not be smooth if the spring back magnitude is large and the transition is small. Method 6 The smoothness and the transition region of the modified surface will depend on the spring back magnitude and the smoothing factor. If the spring back magnitude is large, the transition region will be increased automatically. On the other hand, the transition region will be smaller if the spring back magnitude is small. At the same time, a larger smoothing factor will result in a smaller transition region. Like method 7, this too is nonlinear. Advantages: The smoothness of the modified surfaces can be controlled. Disadvantages: It is impossible to limit the transition region, and the binder surface (and therefore, draw beads) could change if the spring back is large. Method 3 Similar to Method 6, however, it is a linear method and no iteration is necessary. Method 8 This is an enhanced version of Method 6, and can account for addendum and binder changes. Usually the upper tooling including addendum and binder (in an air draw) are included in the PSIDM definition. Method -8 This method is a modification of Method 8, and is used for trim die nesting (from the drawn panel shape). Methods 1, 2, 4, and 5 These methods are deprecated and may be removed in the future. They are included only for maintaining backwards compatibility. *PARAMETER *CONTROL_FORMING_AUTOPOSITION_PARAMETER *PARAMETER_EXPRESSION *PART_MOVE DOS or linux commands Gravity forming Trimming Springback springback amount < tolerance, or, iterations = 4? Yes Done No Compensation Figure 25-26. Iterative compensation flow chart Preventing Undercut When the draw wall is steep, it is likely that undercut will occur. Since undercut is not acceptable in real world die manufacturing, it must be prevented. The compensation code can automatically detect undercut and issue a warning message. Additionally, LS-DYNA will write a list of undercut elements to a file called blankundercut.tmp so that the user can easily identify which elements may be problematic. If the undercut is limited to only a few elements, it is possible to fix the problem manually. Undercut can be reduced by compensating the spring back only in the punch moving direction (by using a negative scale factor). This method is not 100% reliable and more robust solutions are being studied. Iterative spring back compensation Figure 25-26 is a flow chart showing the iterative spring back compensation algorithm as applied to a typical stamping process. The first stamping process simulation is done following gravity→forming→trimming→spring back (ITERATION 0). The stamping process simulation is set up using eZ-Setup (http://ftp.lstc.com/anonymous/out- going/lsprepost/4.0/metalforming/). With the use of the parameterized automatic tool/blank positioning feature, the process simulation is fully automated (no user intervention required). Based on the calculated spring back amount, tooling geometry is compensated through a compensation run. The stamping process simulation is conducted again, automatically, based on the new compensated tooling, followed by a second tooling compensation (ITERATION 1). Iterations 2, 3, and 4 follow the same pattern. The iteration process is repeated until blank spring back shape conforms to tooling designed intent (target), or until it reaches 4 iterations (typically required to achieve part tolerance). With some shell scripting this iterative loop can be completed automatically. These tools allow the user to toggle between single and double precision version of LS-DYNA. The task of tracking the files involved in the iterative process can be daunting, especially in the advanced stage of the iterations. Figure 25-27 indicate what is written to storage during the process. 1_iter0.dir sub-directories 1_gravity.dir 2_form.dir sim_forming_mesh.k 3_trim.dir dynain and geocur.trm rigid.new 4_spbk.dir dynain 5_comp.dir geotrm.new disp.tmp geotrm.new rigid.new 2_iter1.dir sub-directories 1_gravity.dir 2_form.dir 3_trim.dir dynain 4_spbk.dir dynain 5_comp.dir disp.tmp geotrm.new rigid.new 5_iter4.dir 4_iter3.dir rigid.new 3_iter2.dir sub-directories sub-directories geotrm.new sub-directories 1_gravity.dir 2_form.dir 3_trim.dir 4_spbk.dir rigid.new geotrm.new 1_gravity.dir 2_form.dir 3_trim.dir dynain 4_spbk.dir dynain 5_comp.dir 1_gravity.dir 2_form.dir 3_trim.dir dynain 4_spbk.dir dynain 5_comp.dir disp.tmp geotrm.new rigid.new Figure 25-27. File structure for compensation An input deck defining a spring back compensation model is given below. The keyword file blank0.k includes node and element information of the blank shape before spring back (after forming and trimming) with adaptive constraints (if exist). The keyword file spbk.k includes node and element information of the blank after spring back, with adaptive constraints (if they exist). The blank shapes before and after springback (blank0.k and spbk.k) may be based on either the original die design (ITER0), or based on an intermediate compensated die design (say the nth iteration). The keyword file reference0.k is the blank shape before spring back for iteration 0 (ITER0). This file is blank0.k and should not change from iteration to iteration. For iteration 0 the file reference1.k is also the same as blank0.k, but for iteration 1 refereince1.k should be the disp.tmp generated from the compensation calculation during iteration 0 and so on and so forth for the subsequent iterations. The keyword input tools.k must contain the mesh information for all of the stamping tools in their home positions. Compensated tools will be written to rigid.new with the original constant gap being maintained among the tools. During the baseline calculation, iteration 0, a keyword file called geocur.trm, generated during a LS-DYNA trimming simulation based on trimming curve input (usually in IGES format), is used for keyword *INCLUDE_COMPENSATION_TRIM_CURVE. In the compensation run of the ITER1, geocur.trm is used to generate new trim curves called geotrm.new, which conforms to the current compensated tools; and this new mapped trim curves are used for the ensuing ITER2, so on and so forth. The new trim file, geotrm.new is also is also in keyword format and contains a *DEFINE_CURVE_TRIM_3D card. In the example below models a three-piece air draw process. The upper die cavity (including binder) has a part ID 2, which is included in the part set ID 1 and is used for variable PSIDM. Method 8 will compensate all the tools included in file tools.k based on compensated shape for the upper cavity. *KEYWORD $---+----1----+----2----+----3----+----4----+----5----+----6----+----7----+-- *INTERFACE_COMPENSATION_NEW $ METHOD SL SF ELREF PSIDm UNDRCT ANGLE NLINEAR 8 10.000 1.000 0 1 0 0.0 1 *INCLUDE_COMPENSATION_BLANK_BEFORE_SPRING BACK blank0.k *INCLUDE_COMPENSATION_BLANK_AFTER_SPRINBACK spbk.k *INCLUDE_COMPENSATION_DESIRED_BLANK_SHAPE reference0.k *INCLUDE_COMPENSATION_COMPENSATED_SHAPE reference1.k *INCLUDE_COMPENSATION_CURRENT_TOOLS tools.k *INCLUDE_COMPENSATION_TRIM_CURVE geocur.trm *SET_PART_LIST $ PSID 1 $ PID 2 $---+----1----+----2----+----3----+----4----+----5----+----6----+----7----+-- *END NUMISHEET 2005: In Figure 25-28, the NUMISHEET 2005 cross member is compensated following the flow chart. In two iterations the spring back is reduced from 13mm to 1.7mm. Further iterations will reduce the part deviation down to a specific design target. Typically, four iterations are needed. Iterative compensation applied during die construction The blank shape after spring back can be obtained from the actual experimental shape of the spring back panel, if available. For example, in hard tool construction, the trimmed panel can be scanned using white light technology and the panel shape can be written to an STL file. The STL format can be easily converted to LS-DYNA keyword format and the trimmed panel can be used as a rigid tool onto which the baseline (ITER0) trimmed panel (deformable) can be “pushed” using element normal pressure, and using *CONTROL_IMPLICIT_FORMING type 1. In this scenario, the adaptive refinement is turned off to maintain the one-to-one correspondence of the elements and nodes information. An advantage of this method is that the spring back shape used for compensation will be exactly the same as the actual panel spring back, therefore the best tooling compensation result is expected. An example of such is shown in Figures 25-29 and 25-30. Compensation of localized regions Compensation of a localized tooling region is possible, with the keyword *INCLUDE_- COMPENSATION_CURVE, by incorporating the following lines into the above example inputs: *INCLUDE_COMPENSATION_CURVE curves.k The file curves.k defines the two enclosed “begin” and “end” curves using *DEFINE_- CURVE_COMPENSATION_CONSTRAINT_BEGIN/END. More explanations can be found in the corresponding keyword manual entries. In Figure 25-31, the NUMISH- EET’05 decklid inner is compensated locally in the horizontal area above the backlite. Tangency of the compensated tool is maintained at the “End Curve” as shown in the section A-A. Also shown in Figure 25-32 includes color contours of part-separation distance throughout the iterations between compensated panel and the target design intent. Part tolerance is achieved in two iterations. Accelerated spring back compensation (ASC) The option ACCELERATOR can be used in conjunction with *INCLUDE_COMPENSA- TION, with options ORIGINAL_DYNAIN and SPRING BACK_INPUT to compensate spring back with a faster convergence rate and a simplified user interface. A complete example is provided below. The example uses a spring back input file spbk.dyn, and a trimmed panel, with file name case20trimmed.dynain (including all stress and strain tensors and adaptive constraints). The variable ISTEPS is increased from 0 to 3, representing 3 compensation iterations. ISTEPS = 0 represents the baseline spring back simulation (ITER0); while ISTEPS = 1, 2, 3 represent the compensation iterations. This feature requires the user to change only one variable (ISTEPS), and then submit the same input file to continue the next iteration. Many scratch files, including a file named acceltmp.tmp, will be generated. Do not delete them. They are used to pass data between steps. A file, compensation.info, is generated and updated after each ISTEPS calculation. It contains iteration information, including maximum deviations in the 𝑥, 𝑦, and 𝑧 directions. When the maximum deviation is within the tolerances specified in the TOLX, TOLY, and TOLZ fields, a message appears in the file indicating the compensation iterations have converged, along with a message bootstrapping the next step. A file spbk.new is generated in the same directory and is used by the *INCLUDE_COMPENSATION_BLANK_AFTER_- SPRING BACK keyword with the scale factor for the tool compensation set to one. After the compensation, a verification calculation may be needed. *KEYWORD *INTERFACE_COMPENSATION_NEW_ACCELERATOR $ ISTEPS TOLX TOLY TOLZ OPTION 3 0.20 0.20 0.2 1 *INCLUDE_COMPENSATION_ORIGINAL_DYNAIN ./case20trimmed.dynain *INCLUDE_COMPENSATION_SPRING BACK_INPUT ./spbk.dyn *END Currently, mesh coarsening and checking are not supported in the accelerated mode. Also, the dynain file from the previous die process is not necessary. An example of this feature is shown for a simple channel type of draw (one-half model) in Figure 25-33, which converged in three iterations; while four iterations were needed for the non-accelerated compensation. Line die compensation The option MULTI_STEPS can be used together with *INCLUDE_COMPENSATION_- COMPENSATED_SHAPE_NEXT_STEP to enable compensation of tools for the next die process. An example is given below. In this example the target blank, named reference0.tmp, and the current tool named rigid.tmp come from the first die process. The disp.tmp file comes from the compensation in the second die process step. For example, a flanging die compensation can be a second die process step, preceded by a redraw die process as the first die process step. *KEYWORD *INTERFACE_COMPENSATION_NEW_MULTI_STEPS $---+----1----+----2----+----3----+----4----+----5----+----6----+----7----+----8 $ METHOD SL SF ELREF PSID UNDRCT ANGLE NLINEAR 8 6.000 1.00 1 1 0 0 1 *INCLUDE_COMPENSATION_DESIRED_BLANK_SHAPE reference0.tmp *INCLUDE_COMPENSATION_COMPENSATED_SHAPE_NEXT_STEP disp.tmp *INCLUDE_COMPENSATION_CURRENT_TOOLS rigid.tmp *SET_PART_LIST $ PSID 1 $ PID 2 *END Compensation of trim dies (trim die nesting) The trim die can be compensated using the drawn panel’s springnack shape when METHOD is set to -8. In the example below, which is also shown in Figure 25-34, the draw panel, state1.k, is taken as the blank before spring back, and, draw panel spring back shape, state2.k, is taken as the blank after spring back. The tool shape for the draw process, drawtool.k, is used as the current tool. After the simulation, LS-DYNA will create a compensated tool named rigid.new, which can be used for the trim die shape. *KEYWORD $---+----1----+----2----+----3----+----4----+----5----+----6----+----7----+----8 *INTERFACE_COMPENSATION_NEW $ METHOD SL SF ELREF PSID UNDRCT ANGLE NLINEAR -8 10.000 1.000 2 1 0 0.0 1 *INCLUDE_COMPENSATION_BLANK_BEFORE_SPRINGBACK state1.k *INCLUDE_COMPENSATION_BLANK_AFTER_SPRINGBACK state2.k *INCLUDE_COMPENSATION_DESIRED_BLANK_SHAPE ref0.tmp *INCLUDE_COMPENSATION_COMPENSATED_SHAPE ref1.tmp *INCLUDE_COMPENSATION_CURRENT_TOOLS drawtool.k *INCLUDE_COMPENSATION_TRIM_CURVE orginaltrim.k *SET_PART_LIST $ PSID 1 $ PID 3 $---+----1----+----2----+----3----+----4----+----5----+----6----+----7----+----8 *END Local smoothing of tooling mesh: The option LOCAL_SMOOTH can be used, along with a few more keywords, to smooth and restore the distorted tooling mesh after iterative compensation. In the example below, the keyword *INCLUDE_COMPENSATION_ORIGINAL_RIGID_- TOOL includes an original tool, rigid.tmp, which has a good and smooth mesh. The keyword *INCLUDE_COMPENSATION_NEW_RIGID_TOOL includes a compensated tool, rigidnew.bad, which could have a distorted mesh arising from the reasons listed in the “Purpose” section of this keyword. The last keyword *SET_NODE_LIST_SMOOTH defines a node set in and surrounding a distorted local area in the distorted mesh. Each node set defines a region needing smoothing. The node set should not include any boundary nodes of the tooling parts, otherwise position of the tooling may be altered undesirably. Smoothed tooling is stored in a file called rigid.new. In this example method 7 is active, the variable ELREF is set to 2, and PSID left as undefined. Note also the *INCLUDE keyword is not supported here. For example, *SET_NODE_LIST_SMOOTH must not be in a separate file and included in the main input file. *KEYWORD *INTERFACE_COMPENSATION_NEW_LOCAL_SMOOTH $ METHOD SL SF ELREF PSID UNDRCT ANGLE NLINEAR 7 10.000 1.000 2 0 0.0 1 *INCLUDE_COMPENSATION_ORIGINAL_RIGID_TOOL rigid.tmp *INCLUDE_COMPENSATION_NEW_RIGID_TOOL rigidnew.bad *SET_NODE_LIST_SMOOTH 1 61057 61058 61059 61060 61061 61062 61063 61064 ... *SET_NODE_LIST_SMOOTH 2 56141 56142 56143 56144 56145 56146 56147 56148 ... *END In an example shown in Figures 25-35 and 25-36, smoothing of the local mesh is performed in the draw bead area of the NUMISHEET 2005 cross member. In this case the die gap is not maintained throughout the tooling surface. Typically this happens in the draw bead regions when male beads have lower bending radii (missing upper radii) and female beads have only upper bending radii (missing lower radii). Two node sets are defined for local areas of left and right female draw beads (Figure 25-37), which needed smoothing. It is important to include in the node sets some of the nodes on the relatively flat portion of the binder immediately off the bend radii. Smoothed results show original distorted meshes on the lower beads corner areas are corrected and is satisfactory, Figure 25-38. In another example, a corner of a flanging die on a fender outer is being smoothed. The mesh becomes distorted after a few compensation iterations, as shown in Figure 25-39. In Figure 25-40, the result of local smoothing is shown, and the improvement is remarkable. Compensation with symmetric boundary condition A keyword example is provided in the manual pages related to *INCLUDE_COMPEN- SATION_{OPTION}. Global compensation using the original tool mesh For some tooling meshes, the compensated die surfaces will be distorted. The keyword option *INCLUDE_COMPENSATION_ORIGINAL_TOOL causes the compensation code to use the original tooling mesh (starting in the second compensation) to extrapolate the addendum and binder in the compensated tooling surfaces. This minimizes the accumulative error, compared with using the last compensated tooling mesh, and therefore is a preferred method. A complete keyword example is included below. In it, part ID 3 (included in part set ID 1) is being compensated after ITERATION #3 (ITER3), using method #8, with a scale factor of 0.5. The dynain files from the trimmed ITER3 is taken as the “BEFORE” state and the dynain file from the springback calculation is taken as the “AFTER” state. The “DESIRED” blank shape is given by the dynain is from the trimmed ITER0 output. The “COMPENSATED_SHAPE” is taken from the disp.tmp file of the last compensation run. “CURRENT_TOOL” is also from last compensation iteration. The “ORIGINAL_TOOL”, is taken from the tool mesh in ITER0. Updated trim curves geotrm.new are taken from the mapped trim lines of last compensation. It should be noted that, in an automatic compensation-loop calculation, as shown in the path of the input files, input files disp.tmp, rigid.new, and geotrm.new, taken from the default file names of the previous compensation, should not be in the same directory as the current compensation run, as these files will be overwritten. *KEYWORD $---+----1----+----2----+----3----+----4----+----5----+----6----+----7----+----8 *INTERFACE_COMPENSATION_NEW $ METHOD SL SF ELREF PSID UNDRCT ANGLE NLINEAR 8 10.000 0.500 2 1 1 0.0 1 *INCLUDE_COMPENSATION_BLANK_BEFORE_SPRINGBACK ../7_iter3.dir/2_trim.dir/dynain *INCLUDE_COMPENSATION_BLANK_AFTER_SPRINGBACK ../7_iter3.dir/3_spbk.dir/dynain *INCLUDE_COMPENSATION_DESIRED_BLANK_SHAPE ../1_iter0.dir/2_trim.dir/dynain *INCLUDE_COMPENSATION_COMPENSATED_SHAPE ../6_compensation.dir/disp.tmp *INCLUDE_COMPENSATION_CURRENT_TOOLS ../6_compensation.dir/rigid.new *INCLUDE_COMPENSATION_ORIGINAL_TOOLS ../1_iter0.dir/sim_forming_mesh.k *INCLUDE_COMPENSATION_TRIM_CURVE ../6_compensation.dir/geotrm.new *SET_PART_LIST $ PSID 1 $ PID 3 $---+----1----+----2----+----3----+----4----+----5----+----6----+----7----+----8 *END Updating compensated tool with small amount of part shape change Often times a part will have some small amount of shape change as a result of a product change. If the amount of shape change does not significantly alter the spring back results, the compensated tools can be updated with the part mesh (inside the trim lines) or formed blank shape without going through another iterative compensation loop. This is accomplished using the PART_CHANGE option. Within the specified MAX- GAP, compensated tool shape can be updated. Changes to geometry involving sharp corners and transition with no fillet are not permissible. A complete keyword example is provided below, where a maximum gap of 5mm is specified between the original shape and modified product shape. The updated part file name is updatepart.tmp and output file for the new rigid tool is newrigid.k. *KEYWORD *INTERFACE_COMPENSATION_NEW_PART_CHANGE $ MAXGAP 5.0 *INCLUDE_COMPENSATION_DESIRED_BLANK_SHAPE ../1_iter0.dir/2_trim.dir/dynain *INCLUDE_COMPENSATION_COMPENSATED_SHAPE ../6_compensation.dir/disp.tmp *INCLUDE_COMPENSATION_CURRENT_TOOLS ../6_compensation.dir/rigid.new *INCLUDE_COMPENSATION_UPDATED_BLANK_SHAPE ./updatedpart.tmp *INCLUDE_COMPENSATION_UPDATED_RIGID_TOOL $ file name to output the new rigid tools ./newrigid.k *END Option REFINE_RIGID: rigid tool mesh refinement for a better convergence The following keyword example refines and breaks the elements in the original tool mesh file rigid.new along provided trim curves trimcurve106.k, defined using the keyword *DEFINE_CURVE_TRIM_3D. The refined rigid tool mesh will be output as rigid_refined.tmp, which can be used to start the iterative springback compensation process. *KEYWORD *INTERFACE_COMPENSATION_NEW_REFINE_RIGID rigid.new trimcurve106.k *END Reference: The manual pages related to *INCLUDE_COMPENSATION_{OPTION} can be further referenced for details. Revision Information: This keyword requires double precision executable. The option of ACCELERATOR is available starting in Revision 61264. The option of MULTI_STEPS is available starting in Revision 61406. The option of LOCAL_SMOOTH is available starting in Revision 73850. The keyword option *INCLUDE_COMPENSATION_ORIGINAL_TOOL is available starting in Revision 82701. The keyword option PART_CHANGE is available starting in Revision 82698. The REFINE_RIGID option is available starting in Revision 113089. Nominal Surface ■ ITERATION 0 ■ Max. springback 13mm on flanges Trim Panel Springback ■ ITERATION 1 ■ Springback reduced to < 3.5mm Springback Covergence (mm) 15.0 10.0 5.0 0.0 ■ ITERATION 2 ■ Springback reduced to < 1.7mm Max Deviation 1.7m ITER0 ITER1 ITER2 ■ Compensation convergence history Symmetry Plane Upper Die Cavity Sheet Blank Trim Lines Lower Binder Lower Post Drawn Panel 2005 NUMISHEET Cross Member Model Drawn Panel and Trim Lines Figure 25-28. Xmbr(red – springback, blue – design intent) Iterative springback compensation on NUMISHEET’05 Scan data from (STL) "Pushed in" blank Figure 25-29. A trimmed panel “pushed” onto the scan data (rigid body). Figure 25-30. Section showing the “push” results – before and after. Begin curve Transition region End curve Figure 25-31. Two curves defining a localized area of a decklid inner. Section A-A ITER0 ITER1 ITER2 Distance to target (mm) 3.5 3.0 2.5 2.0 1.5 1.0 0.5 0.0 Figure 25-32. Iterative compensation for a localized (backlite) region. Distance to target (mm) with ISTEP=0~3, 1 verification run 0.5 0.4 0.3 0.2 0.1 0.0 ITER0 trim panel ITER0 springback Original tools Accelerated Springback Compensation Figure 25-33. Accelerated Springback Compensation. rigid.new (compensated draw tools for trim die) drawtool.k state1.k (drawn panel) state2.k (drawn panel springback) Figure 25-34. Trim die compensation with drawn panel springback shape. Figure 25-35. The NUMISHEET 2005 cross member. Figure 25-36. Multiple sections cut on the lower binder. Node set 1 Node set 2 Figure 25-37. Local smoothing - two node sets defined including some nodes on the relatively flat binder area for both left and right draw beads. Original distorted Smoothed Figure 25-38. Comparison between original and smoothed tooling mesh. Figure 25-39. Original distorted tooling mesh. Figure 25-40. Smoothed tooling mesh. *INTERFACE_COMPONENT_FILE Purpose: Allow for the specification of the file where the component interface data should be written, and the optional use of a new binary format for that data. Card 1 1 2 3 4 5 6 7 8 Variable Type Default Optional Card. Filename A80 none Card 2 1 2 3 4 5 6 7 8 Variable Format Type Default I 2 VARIABLE DESCRIPTION FNAME Name of the file where the component data will be written FORMAT File format to use: EQ.1: Use old binary file format EQ.2: Use new LSDA file format Remarks: If Z = is used on the command line, this card will be ignored. If this card is in effect, the new LSDA file format is the default format to be used. The new format has certain advantages, and one possible drawback: 1. It allows for the use of the_TITLE modifier on all *INTERFACE_COMPONENT inputs, so that subsequent *INTERFACE_LINKING cards can refer to compo- nents by a user specified ID. 2. 3. It is fully portable between machines with different precision and byte order. It maintains the full precision of the coordinate vector. The internal coordinate vector has been in double precision for quite some time, even for single preci- sion executables. The old binary format writes 32 bit data for single precision executables, losing some precision in the process. 4. Because of the maintained precision, the new format files will be significantly larger when running in single precision. Of course, the new file format cannot be used for subsequent analysis with older versions of LS-DYNA, particularly those with a Product ID less than 50845. Executables which can read the new format for *INTERFACE_LINKING analysis will automatically detect whether the new or old format is in use. *INTERFACE_COMPONENT_OPTION1_{OPTION2} Available values for OPTION1 include: NODE SEGMENT OPTION2 only allows the value: TITLE Purpose: Create an interface for use in subsequent linking calculations. This command applies to the first analysis for storing interfaces in the interface file specified either by “Z=isf1” on the execution line or by the *INTERFACE_COMPONENT_FILE command. The output interval used to write data to the interface file is controlled by OPIFS on *CONTROL_OUTPUT. If OPIFS is not specified, the interval defaults to 1/10th the value of DT specified in *DATABASE_BINARY_D3PLOT. This capability allows the definition of interfaces that isolate critical components. A database is created that records the motion of the interfaces. In later calculations the isolated components can be reanalyzed with arbitrarily refined meshes with the motion of their boundaries specified by the database created by this input. The interfaces defined here become the masters in the tied interface options. Each definition consists of a set of cards that define the interface. Interfaces may consists of a set of segments for later use with *INTERFACE_LINKING_SEGMENT, an ordered line of nodes for use with *INTERFACE_LINKING_EDGE, or an unordered set of nodes for use with *INTERFACE_LINKING_NODE. Title Card. Additional card for TITLE keyword option. Card 1 Variable 1 ID Type I Default none 2 3 4 5 6 7 8 Title A70 None VARIABLE DESCRIPTION ID Title LS-DYNA R10.0 ID for this interface in the linking file Card 2 1 2 3 4 5 6 7 8 Variable SID CID NID Type I I I VARIABLE DESCRIPTION Set ID, see *SET_NODE or *SET_SEGMENT. Coordinate system ID Node ID SID CID NID Remarks: CID and NID are optional. If CID appears, the transformation matrix for this coordinate system is written to the linking file at each output state. If NID appears, the displacement of this node is also written to the file. This information is then available to be used by the *INTEFACE_LINKING_NODE_LOCAL. If either of these is non-zero, then the linking file will be written in the LSDA format, as the old format cannot support this optional output. If the old style binary format is used for the linking file then the ID values are ignored and all components are numbered according to their input order, starting from 1. *INTERFACE Purpose: Define the failure models for bonds linking various discrete element (DE) parts within one heterogeneous bond (*DEFINE_DE_HBOND). 2 3 4 5 6 7 8 Card 1 Variable 1 IID Type I Default none Bond Definition Cards. For each bond definition, include an additional card. This input ends at the next keyword (“*”) card. Optional 1 2 3 4 5 6 7 8 Variable PID1 PID2 PTYPE1 PTYPE2 FRMDL FRGK FRGS DMG Type I I I I Default none none none none I 1 F F F none none 1.0 VARIABLE DESCRIPTION IID PID1 Interface ID. All interfaces should have a unique ID First part ID. VARIABLE PID2 DESCRIPTION Second part ID. PID1 and PID2 define the bonds that this fracture model is applied to. There are three combinations as Case a: PID1.EQ.0 This is the default model for all bonds, overriding the de- fault model defined in Card 2 of *DEFINE_DE_HBOND. Case b: PID1.GT.0 and PID2.EQ.0 This model is applied to the bonds within part PID1, instead of the default model. Case c: PID1.GT.0 and PID2.GT.0 This model is applied to the bonds between parts PID1 and PID2 only, but not to those within part PID1 or part PID2 (as in case b). Notes: 1. The default fracture model is applied to all parts that are not specified in case b. 2. The fracture model of the part with a smaller part id is applied to the bonds between two different parts if not spec- ified in case c. PTYPE1 First part type: EQ.0: DES part set EQ.1: DES part PTYPE2 Second part type: EQ.0: DES part set EQ.1: DES part FRMDL Fracture model. (same as FRMDL in Card2 of keyword *DEFINE_- DE_HBOND.) FRGK FRGS DMG Fracture energy release rate for volumetric deformation. (same as FRGK in Card2 of keyword *DEFINE_DE_HBOND.) Fracture energy release rate for shear deformation. (same as FRGS in Card 2 of keyword *DEFINE_DE_HBOND.) Continuous damage development. (same as DMG in Card 2 of keyword *DEFINE_DE_HBOND.) INTERFACE_DE_HBOND EXAMPLE: $$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ $ $ *INTERFACE_DE_HBOND $ $$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ $ Using DE_HBOND to bond 4 parts with different failure models $ *SET_PART_LIST_TITLE DES BOND PARTS $ $...>....1....>....2....>....3....>....4....>....5....>....6....>....7....>....8 $ sid da1 da2 da3 da4 1 $ id1 id2 id3 id4 101 102 103 104 *SET_PART_LIST_TITLE DES HBOND SUB PARTS $ $...>....1....>....2....>....3....>....4....>....5....>....6....>....7....>....8 $ sid da1 da2 da3 da4 2 $ id1 id2 103 104 *INTERFACE_DE_HBOND $ $...>....1....>....2....>....3....>....4....>....5....>....6....>....7....>....8 $ iid 1 $ pid1 pid2 ptype1 ptype2 frmdl frgk frgs dmg 101 0 1 0 1 1.0E1 1.0E1 1.0 2 0 0 0 1 1.0E3 1.0E3 1.0 102 103 1 1 2 1.0E2 1.0E2 1.0 $ *DEFINE_DE_HBOND $ $...>....1....>....2....>....3....>....4....>....5....>....6....>....7....>....8 $ sid stype bdform idim 1 2 2 3 $ pbk_sf pbs_sf frgk frgs bondr alpha dmg frmdl 1 1 1.0E0 1.0E0 2.5 0.01 1.0 1 $ precrk cktype itfid 0 0 1 $$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ $ the fracture models for the bonds within each part are determined as $ $ pid1 pid2 frgk comments $ 101 101 1.0E1 Line 1 in the interface card $ 102 102 1.0E0 default (defined in hbond card) $ 103 103 1.0E3 Line 2 in the interface card $ 104 104 1.0E3 Line 2 in the interface card $ $ for the bonds between two parts: $ 101 102 1.0E1 taken from Part 101 (smaller part id) $ 101 103 1.0E1 taken from Part 101 (smaller part id) $ 101 104 1.0E1 taken from Part 101 (smaller part id) $ 102 103 1.0E2 Line 3 in the interface card $ 102 104 1.0E0 taken from Part 102 (smaller part id) $ 103 104 1.0E3 taken from Part 103 (smaller part id) $$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ *INTERFACE_LINKING_DISCRETE_NODE_OPTION Available options include: NODE SET Purpose: Link node(s) to an interface in an existing interface file. This link applies to all element types. The interface file is specified using *INTERFACE_LINKING_FILE or by including “L=filename” on the execution line. With this command, nodes in a node set must be given in the same order as they appear in the interface file. This restriction does not apply to the more recent keyword *INTER- FACE_LINKING_NODE_…. Card 1 1 2 3 4 5 6 7 8 Variable NID/NSID IFID Type I I VARIABLE NID DESCRIPTION Node ID or Node set ID to be moved by interface file, see *NODE or *SET_NODE. IFID Interface ID in interface file. *INTERFACE Purpose: Link a series of nodes to an interface in an existing interface force file. The including interface file “L=filename” on the execution line. is specified using *INTERFACE_LINKING_FILE or by Card 1 2 3 4 5 6 7 8 Variable NSID IFID Type I I VARIABLE DESCRIPTION Node set ID to be moved by interface file. Interface ID in interface file. NSID IFID Remarks: The set of nodes defined will be constrained to follow the movement of the interface IFID, which should correspond to a curve output on a previous analysis via *INTER- FACE_COMPONENT_NODE. The order of the nodes in the first analysis is important. The nodes, in the order specified in the first analysis, represent a curve. Each node in set NSID will be tied to the point on the curve nearest to its initial position, and then will be constrained to follow that point on the curve for the duration of the analysis. This option is intended to be used with beam or shell elements, as both translational and rotational degrees of freedom are constrained. *INTERFACE_LINKING_FILE Purpose: Allow for the specification of the file from which the component interface data should be read. Card 1 1 2 3 4 5 6 7 8 Variable Type Default Filename A80 none VARIABLE DESCRIPTION FNAME Name of the file from which the component data will be read Remarks: If L= is used on the command line, this card will be ignored. There is no option to specify the file format, as the file format is automatically detected. *INTERFACE_LINKING_NODE_OPTION Available options include: SET LOCAL SET_LOCAL Purpose: Link nodes(s) to an interface in an existing interface file. This link applies to all element types. The interface file is specified using *INTERFACE_LINKING_FILE or by including “L=filename” on the execution line. Node/Set ID Card. Include as many cards as desired. Input ends at the next keyword (“*”) card. Card 1 1 2 Variable NID/NSID IFID Type I I 3 FX I 4 FY I 5 FZ I VARIABLE DESCRIPTION 6 7 8 NID IFID FX FY FZ Node ID or Node set ID to be moved by interface file, see *NODE or *SET_NODE. Interface ID in interface file. The ID of a *DEFINE_FUNCTION which determines the 𝑥 direction displacement scale factor The ID of a *DEFINE_FUNCTION which determines the 𝑦 direction displacement scale factor The ID of a *DEFINE_FUNCTION which determines the 𝑧 direction displacement scale factor Card 2. This card appears after Card 1 when the_LOCAL option is used Card 2 1 2 3 4 5 6 7 8 Variable LCID LNID USEC USEN Type I I I I VARIABLE DESCRIPTION Local coordinate system ID for transforming displacements. Local node ID for transforming displacements 0/1 flag to indicate the use of the coordinate system in the linking file during displacement transformation 0/1 flag to indicate the use of the node displacement in the linking file during displacement transformation. LCID LNID USEC USEN Remarks: The set of nodes is constrained to follow the displacement of the interface having ID IFID in the linking file. Note that the linking file is usually generated by the *INTER- FACE_COMPONENT_NODE kekyword in a previous analysis. The order of the nodes is not important. Each node in set NID will be tied to the nearest node in IFID using a bucket sort during the initialization phase. Nodes not found are reported and subsequently not constrained. Translational degrees of freedom are constrained. If the constrained analysis has rotational degrees of freedom, then the rotation degrees of freedom will be likewise constrained and the linking file must include rotational degrees of freedom. The displacements in the linking file can be scaled upon input so that 𝐮constrained = 𝑓FX(… ) ⎡ ⎢ ⎣ 𝑓FY(… ) ⎤ ⎥ 𝑓FZ(… )⎦ 𝐮linking file where 𝑓FX(… ) is the *DEFINE_FUNCTION function having ID FX and so on. When a scaling function is not specified the corresponding component is imported unscaled as if the scaling function had a constant value of unity. These functions may take either 0, 1, 3, or 4 input arguments. The functions FX, FY, and FZ may be different and they may take different numbers of arguments. The data passed into the scaling function depends on the number of arguments that the function takes and the possibilities can be broken down into four cases: 1. 2. 3. 4. 0 variables. A function taking no inputs is evaluate constant over space and time. LS-DYNA evaluates such a function at the start of the calculation and uses that value for the duration of the run. 1 varriables. LS-DYNA passes in the simulation time at each step and the resulting value is applied to all nodes in the set. 3 varriables. LS-DYNA passes in the initial position of each constrained node as an (𝑥, 𝑦, 𝑧) triple at the start of the calculation and then uses the result for the duration of the run. 4 varriables. LS-DYNA passes in the current simulation time and the initial position of each of the constrained nodes as an (𝑥, 𝑦, 𝑧, 𝑡) tuple. This function is updated at each time step. Using scaling functions of 4 variables may result in a performance penalty as each function must be evaluated for every slave node every cycle. If time dependent scaling functions are used, then the constrained nodes must start with coordinates identical to the constraining nodes in the linking file. The LOCAL option and the values of the LCID, LNID, USEC, USEN flags, which was designed in conjunction with Honda R&D Co., Ltd., allow for the interface displacements to be transformed in various ways. By default, the scale factors FX, FY, FZ act on the nodal displacements in the global coordinate system of the constrained calculation. This may be undesirable depending on how the global coordinate system of the linked calculation is defined. The most general transformation rule is: 𝐮constrained = 𝐐2 𝑓FX(… ) ⎡ ⎢ ⎣ 𝑓FY(… ) ⎤ ⎥ 𝑓FZ(… )⎦ 𝐐𝟏(𝐮linked − 𝐜𝟏) − 𝐜𝟐 where, 𝐜1 = The displacement of the NID node in the linking file 𝐜𝟐 = The displacement of node LNID 𝐐1 = Rotation into the local coordinates of the linking file 𝐐2 = Rotation into the local coordinate system, if unset the inverse of 𝐐1 If USEC = 0, then 𝐐1 is the identity rotation and any coordinate system in the linking file is ignored. If USEN = 0, then 𝐜1 is set to 0 and NID in the linking file is ignored. *INTERFACE_LINKING_SEGMENT Purpose: Link segments to an interface in an existing interface file. The interface file is specified using *INTERFACE_LINKING_FILE or by including “L=filename” on the execution line. Segment Set ID Card. Include as many cards as desired. Input ends at the next keyword (“*”) card. Card 1 1 2 3 4 5 6 7 8 Variable SSID IFID Type I I VARIABLE DESCRIPTION Segment set to be moved by interface file. Interface ID in interface file. SSID IFID Remarks: The set of segments defined will be constrained to follow the movement of the interface IFID, which should correspond to an interface output on a previous analysis using the *INTERFACE_COMPONENT_SEGMENT keyword. The behavior will be the same as if set SSID is the slave side of a *CONTACT_TIED_SURFACE_TO_SURFACE with IFID as the master. Translational movement will be constrained, but not rotations. *INTERFACE_SPRINGBACK_OPTION1_OPTION2 Available options included for OPTION1 are: LSDYNA NASTRAN SEAMLESS EXCLUDE and for OPTION2: THICKNESS NOTHICKNESS See Remark 1. Purpose: Define a material subset for an implicit springback calculation in LS-DYNA and any nodal constraints to eliminate rigid body degrees-of-freedom. Card 1 1 2 3 4 5 6 7 8 Variable PSID NSHV FTYPE FTENSR NTHHSV INTSTRN Type I I I I I I Irregular Optional Card. The keyword reader will interpret the card following Card 1 as new optional Card 2 if the first column of the card is occupied by the string “OPTCARD”. Otherwise, it is interpreted as first Node Card, see below. Card 2 1 2 3 4 5 6 7 8 Variable OPTC SLDO NCYC FSPLIT NDFLAG Type A I I I Node Cards. Define a list of nodal points that are constrained for the springback. This section is terminated by an “*” indicating the next input section. Card 1 Variable NID Type I 2 TC F 3 RC F 4 5 6 7 8 VARIABLE DESCRIPTION PSID NSHV Part set ID for springback, see *SET_PART. Number of shell or solid history variables (beyond the six stresses and effective plastic strain) to be initialized in the interface file. For solids, one additional state variable (initial volume) is also written. If NSHV is nonzero, the element formulations, unit system, and constitutive models should not change between runs. If NHSV exceeds the number of integration point history variables required by the constitutive model, only the number required is written; therefore, if in doubt, set NHSV to a large number. FTYPE File type: EQ.0: ASCII, EQ.1: binary EQ.2: both ASCII and binary. EQ.3: LSDA format (for LSDYNA only) EQ.10: ASCII large format EQ.11: binary large format EQ.12: both ASCII and binary large format FTENSR Flag for dumping tensor data from the element history variables into the dynain file. EQ.0: Don’t dump tensor data from element history variables EQ.1: Dump any tensor data from element history variables into the dynain file in GLOBAL coordinate system. Cur- rently, only Material 190 supports this option. VARIABLE DESCRIPTION NTHHSV Number of thermal history variables. INTSTRN Output of strains at all integration points of shell element is requested, see also *INITIAL_STRAIN_SHELL. SLDO Output of solid element data as EQ.0: *ELEMENT_SOLID, or EQ.1: *ELEMENT_SOLID_ORTHO. NCYC Number of process cycles this simulation corresponds to in the simulation of wear processes, see Remark 6. FSPLIT Flag for splitting of the dynain file (only for ASCII format). EQ.0: dynain file written in one piece. EQ.1: Output is divided into two files, dynain_geo including the geometry data and dynain_ini including initial stress- es and strains. NDFLAG Flag to dump nodes into dynain file. EQ.0: default, dump only sph and element nodes NID TC EQ.1: dump all nodes Node ID, see *NODE. Translational Constraint: EQ.0: no constraints, EQ.1: constrained 𝑥 displacement, EQ.2: constrained 𝑦 displacement, EQ.3: constrained 𝑧 displacement, EQ.4: constrained 𝑥 and 𝑦 displacements, EQ.5: constrained 𝑦 and 𝑧 displacements, EQ.6: constrained 𝑧 and 𝑥 displacements. EQ.7: constrained 𝑥, 𝑦, and 𝑧 displacements. VARIABLE DESCRIPTION RC Rotational constraint: EQ.0: no constraints, EQ.1: constrained 𝑥 rotation, EQ.2: constrained 𝑦 rotation, EQ.3: constrained 𝑧 rotation, EQ.4: constrained 𝑥 and 𝑦 rotations, EQ.5: constrained 𝑦 and 𝑧 rotations, EQ.6: constrained 𝑧 and 𝑥 rotations, EQ.7: constrained 𝑥, 𝑦, and 𝑧 rotations. Remarks: 1. NOTHICKNESS Option. The NOTHICKNESS option is available when the keyword’s first option is either LS-DYNA or NASTRAN. With the NOTHICK- NESS option the shell element thickness is not output. 2. Filenames. The file name for the LS-DYNA option is dynain and for NAS- TRAN is nastin. 3. Trimming. Trimming is available for the adaptive mesh, but it requires manual intervention. To trim an adaptive mesh use the following procedure: a) Generate the file, dynain, using the keyword *INTERFACE_SPRING- BACK_LSDYNA. b) Prepare a new input deck including the dynein file. c) Add the keyword *ELEMENT_TRIM to this new deck. d) Add the keyword *DEFINE_CURVE_TRIM to this new deck. e) Run this new input deck with i=input_file_name. The adaptive con- straints are eliminated by remeshing and the trimming is performed. f) In case this new trimmed mesh is needed, run a zero termination time job and output the file generated via the keyword, *INTERFACE_SPRING- BACK_LSDYNA. 4. Temperature. The file new_temp_ic.inc will be created for a thermal solution and a coupled thermal-mechanical solution. The file new_temp_ic.inc is a KEYWORD include file containing new temperature initial conditions for the nodes belonging to the PSID. a) For thermal user materials it is possible to dump thermal history varia- bles. See the NTHHSV field. 5. FTYPE. The choice of format size in option FTYPE is only available for shell stresses and shell history data, see parameter LARGE on *INITIAL_STRESS_- SHELL. For solid and beam elements, always the large format is written to dynain, i.e. LARGE is automatically set to 1 on *INITIAL_STRESS_SOLID and *INITIAL_STRESS_BEAM respectively. 6. NCYC. When simulating wear processes, this represents the number of process cycles this particular simulation corresponds to and *INITIAL_CONTACT_- WEAR cards are generated accordingly in the dynain file (only ascii format supported). Cards will only be generated for nodes in contact interfaces associ- ated with a *CONTACT_ADD_WEAR, and having SPR or MPR set to 2 on the first card on *CONTACT. This wear data is in a subsequent simulation ac- counted for NCYC times when modifying the worn geometry, or alternatively processed in LS-PrePost 7. EXCLUDE. This option is used to limit what data will be output to the LSDYNA dynain file. The input format is completely different, and consists of any number of keyword cards WITHOUT the leading *. These cards and their associated data will not be output. For example: *INTERFACE_SPRINGBACK_EXCLUDE BOUNDARY_SPC_NODE CONSTRAINED_ADAPTIVITY would output all the normal dynain data except for the SPC and adaptive con- straints. The currently recognized keywords that can be excluded are: BOUNDARY_SLIDING_PLANE BOUNDARY_SPC_NODE CONSTRAINED_ADAPTIVITY DEFINE_COORDINATE_NODES DEFINE_COORDINATE_VECTOR ELEMENT_BEAM ELEMENT_SHELL ELEMENT_SOLID INITIAL_STRAIN_SHELL INITIAL_STRAIN_SOLID INITIAL_STRESS_BEAM INITIAL_STRESS_SHELL INITIAL_STRESS_SOLID INITIAL_TEMPERATURE_NODE INITIAL_VELOCITY_NODE NODE REFERENCE_GEOMETRY Remarks for Seamless Springback: When seamless springback is invoked, the solution automatically and seamlessly switches from explicit or implicit dynamic to implicit static mode at the termination time, and continues to run the static springback analysis. Seamless springback can be activated in the original LS-DYNA input deck, or later using a small restart input deck. In this way, the user can decide to continue a previous analysis by restarting to add the implicit springback phase. (Another alternative approach to springback simulation is to use the keyword *INTERFACE_SPRINGBACK_LSDYNA to generate a dynain file after forming, and then perform a second simulation running LS-DYNA in fully implicit mode for springback. See Appendix P for a description of how to run an implicit analysis using LS-DYNA. The implicit springback phase begins when the forming simulation termination time ENDTIM is reached, as specified with the keyword *CONTROL_TERMINATION. Since the springback phase is static, its termination time can be chosen arbitrarily (unless material rate effects are included). The default choice is 2.0 × ENDTIM, and can be changed using the *CONTROL_IMPLICIT_GENERAL keyword; see variables DT0 and NSBS.. Since the springback analysis is a static simulation, a minimum number of essential boundary conditions or Single Point Constraints (SPC's) can be input to prohibit rigid body motion of the part. These boundary conditions can be added for the springback input option on the *INTERFACE_SPRINGBACK_SEAMLESS phase using the keyword above. If no boundary conditions are added with the SEAMLESS option an eigenvalue computation is automatically performed using the Inertia Relief Option to find any rigid body modes and then automatically constrain them out of the springback simulation . This approach introduces no artificial deformation and is recommended for many simulations. An “SPR” option is available for several *CONTROL_IMPLICIT keywords to further control the implicit springback phase. Generally, default settings can be used, in which case the SPR option for *CONTROL_IMPLICIT keywords is not necessary. To obtain accurate springback solutions, a nonlinear springback analysis must be performed. In many simulations, this iterative equilibrium search will converge without difficulty. If the springback simulation is particularly difficult, either due to nonlinear deformation, nonlinear material response, or numerical precision errors, a multi-step springback simulation will be automatically invoked. In this approach, the springback deformation is divided into several smaller, more manageable steps. Two specialized features in LS-DYNA are used to perform multi-step springback analyses. The addition and gradual removal of artificial springs is performed by the artificial stabilization feature. Simultaneously, the automatic time step control is used to guide the solution to the termination time as quickly as possible, and to persistently retry steps where the equilibrium search has failed. By default, both of these features are active during a seamless springback simulation. However, the default method attempts to solve the springback problem in a single step. If this is successful, the solution will terminate normally. If the single step springback analysis fails to converge, the step size will be reduced, and artificial stabilization will become active. Defaults for these features can be changed using the following keywords: • *CONTROL_IMPLICIT_GENERAL, • *CONTROL_IMPLICIT_AUTO, and • *CONTROL_IMPLICIT_STABILIZATION. *INTERFACE_SSI Purpose: This card creates a tied-contact soil-structure interface for use in a transient analysis of a soil-structure system subjected to earthquake excitation. This card allows the analysis to start from a static state of the structure, as well as to read in ground motions recorded on the interface in an earlier analysis. Available options are: <BLANK> OFFSET CONSTRAINED_OFFSET LS-DYNA implements the effective seismic input method [Bielak and Christiano (1984)] for modeling the interaction of a non-linear structure with a linear soil foundation subjected to earthquake excitation. Note that any non-linear portion of the soil near the structure may be incorporated with the structure into a larger generalized structure, but the soil is assumed to behave linearly beyond a certain distance from the structure. The effective seismic input method couples the dynamic scattered motion in the soil, which is the difference between the motion in the presence of the structure and the free- field motion in its absence, with the total motion of the structure. This replaces the distant earthquake source with equivalent effective forces adjacent to the soil-structure interface and allows truncation of the large soil domain using a non-reflecting boundary (e.g. *MAT_PML_ELASTIC) to avoid unnecessary computation. These effective forces can be computed using the free-field ground motion at the soil-structure interface, thus avoiding deconvolution of the free-field motion down to depth. Non-linear behavior of the structure may be modeled by first carrying out a static analysis of the soil-structure system, and then carrying out the transient analysis with only the structure initialized to its static state. Because the transient analysis employs the dynamic scattered motion in the soil, the soil cannot have any static loads only it ― only the structure is subjected to static forces. Consequently, the structure must be supported by the static reactions at the soil-structure interface. Additionally, the soil nodes at the interface must be initialized to be compatible with the initial static displacement of the structure. LS-DYNA will do these automatically if the soil- structure interface is identified appropriately in the static analysis and reproduced in the transient analysis. Thus, soil-structure interaction analysis under earthquake excitation may be carried out in LS-DYNA as follows: 1. Carry out a static analysis of the soil-structure system (e.g. using dynamic relaxation; see *CONTROL_DYNAMIC_RELAXATION), with the soil-structure interface identified using *INTERFACE_SSI_STATIC_ID Optionally, carry out a free-field analysis to record free-field motions on the future soil-structure interface, using either *INTERFACE_SSI_AUX or *INTER- FACE_SSI_AUX_EMBEDDED, for surface-supported or embedded structures respectively. 2. Carry out the transient analysis as a full-deck restart job , with only the structure initialized to its static stress state , and the same soil-structure interface identified using *INTERFACE_- SSI_ID with the same ID as in static analysis: a) The structure mesh must be identical to the one used for static analysis. b) The soil mesh is expected to be different from the one used for static anal- ysis, especially because non-reflecting boundary models may be used for transient analysis. c) The meshes for the structure and the soil need not match at the interface. d) Only the structure must be subjected to static loads, via *LOAD_BODY_- PARTS e) The earthquake ground motion is specified using *LOAD_SEISMIC_SSI, and/or read from motions recorded from a previous analysis using *IN- TERFACE_SSI_AUX or *INTERFACE_SSI_AUX_EMBEDDED. Card 1 Variable 1 ID Type I 2 3 4 5 6 7 8 HEADING A70 Card 2 1 2 3 4 5 6 7 8 Variable STRID SOILID SPR MPR Type I I Default none none I 0 I Card 3 1 Variable GMSET Type I 2 SF F Default none 1. *INTERFACE_SSI 3 4 5 6 7 8 BIRTH DEATH MEMGM F 0. F I 1028 2500000 VARIABLE DESCRIPTION ID Soil-structure interface ID. This is required and must be unique amongst all the contact interface IDs in the model. HEADING A descriptor for the given ID. STRID Segment set ID of base of structure at soil-structure interface. SOILID Segment set ID of soil at soil-structure interface. SPR MPR Include the slave side in the *DATABASE_NCFORC and the *DATABASE_BINARY_INTFOR interface force files: EQ.1: slave side forces included. Include the master side in the *DATABASE_NCFORC and the *DATABASE_BINARY_INTFOR interface force files: EQ.1: master side forces included. GMSET Identifier for set of recorded motions from *INTERFACE_SSI_- AUX or *INTERFACE_SSI_AUX_EMBEDDED SF Recorded motion scale factor. (default = 1.0) BIRTH Time at which specified recorded motion is activated. DEATH Time at which specified recorded motion is removed: EQ.0.0: default set to 1028 MEMGM Size in words of buffer allocated to read in recorded motions *INTERFACE 1. A tied contact interface (*CONTACT_TIED_SURFACE_TO_SURFACE) is created between the structure and the soil using the specified segment sets, with the soil segment set as the master segment set and the structure segment set as the slave. Naturally, the two segment sets should not have merged nodes and can be non-matching in general. However, the area covered by the two surfaces should match. 2. The options OFFSET and CONSTRAINED_OFFSET create the corresponding tied surface-to-surface contact interface. 3. The soil-structure interface ID is assigned as the ID of the generated contact interface. 4. It is assumed that the soil segment set is oriented toward the structure. 5. Multiple soil-structure interfaces are allowed, e.g. for bridge analysis. 6. The recorded motions are read in from a binary file named gmbin by default, but a different filename may be chosen using the option GMINP on the com- mand line . 7. If the motions from *INTERFACE_SSI_AUX or *INTERFACE_SSI_AUX_EM- BEDDED were recorded on a segment set, then the free-field motions on each node in the master segment set of the soil-structure interface are calculated from the nearest segment of the segment set used to record the motions. If, however, the motions were recorded on a node set, then the motions on the master segment set nodes is found by interpolation as is done for *LOAD_SEIS- MIC_SSI. Available options are: <BLANK> NODE *INTERFACE_SSI_AUX Purpose: This card records the motion at a free surface, or on a set of nodes on a free surface, for the purpose of using the recorded motion as a free-field motion in a subsequent interaction analysis using *INTERFACE_SSI. By default, this card records motions on a segment set defining a surface, but can record motions on a node set using the option NODE. Only one of *INTERFACE_SSI_AUX and *INTERFACE_SSI_AUX_- EMBEDDED is to be used for a particular soil-structure interface. Card 1 1 2 3 4 5 6 7 8 Variable GMSET SETID Type I I Default none none VARIABLE GMSET DESCRIPTION Identifier for this set of recorded motions to be referred to in *IN- TERFACE_SSI. Must be unique. SETID Segment set or node set ID where motions are to be recorded. Remarks: 1. The motions on the specified segment set or node set is recorded in a binary file named gmbin by default, but a different filename may be chosen using option GMOUT on the command line . 2. The output interval for the motions may be specified using the parameter GMDT on the *CONTROL_OUTPUT card, with the default value being 1/10-th of the output interval for D3PLOT states. *INTERFACE_SSI_AUX_EMBEDDED_{OPTION1}_{OPTION2} Purpose: This card creates a tied-contact interface and records the motions and contact forces in order to use them as free-field motion and reactions in a subsequent soil- structure interaction analysis using *INTERFACE_SSI, where the structure is embedded in the soil after part of the soil has been excavated. Only one of *INTERFACE_SSI_AUX and *INTERFACE_SSI_AUX_EMBEDDED is to be used for a particular soil-structure interface. Available options for OPTION1 are: <BLANK> OFFSET CONSTRAINED_OFFSET OPTION2 allows an optional ID to be given: ID ID Card. Additional card for ID keyword option. Card 1 Variable 1 ID Type I 2 3 4 5 6 7 8 HEADING A70 Card 2 1 2 3 4 5 6 7 8 Variable GMSET STRID SOILID SPR MPR Type I I I Default none none none I 0 I 0 DESCRIPTION VARIABLE ID Soil-structure interface ID. This is required and must be unique amongst all the contact interface IDs in the model. HEADING A descriptor for the given ID. VARIABLE GMSET DESCRIPTION Identifier for this set of recorded motions to be referred to in *IN- TERFACE_SSI. Must be unique. STRID Segment set ID at base of soil to be excavated. SOILID Segment set ID at face of rest of the soil domain. Include the slave side in the *DATABASE_NCFORC and the *DATABASE_BINARY_INTFOR interface force files: EQ.1: slave side forces included. Include the master side in the *DATABASE_NCFORC and the *DATABASE_BINARY_INTFOR interface force files: EQ.1: master side forces included. SPR MPR Remarks: 1.The motions on the specified segment set or node set is recorded in a binary file named gmbin by default, but a different filename may be chosen using option GMOUT on the command line . 2.The output interval for the motions may be specified using the parameter GMDT on the *CONTROL_OUTPUT card, with the default value being 1/10-th of the output interval for D3PLOT states. *INTERFACE_SSI_STATIC_{OPTION}_ID Purpose: This card creates a tied-contact soil-structure interface in order to record the static reactions at the base of the structure, which are to be used in a subsequent dynamic analysis of the soil-structure system subjected to earthquake excitation. This card is intended to be used with the initial static analysis of the structure subjected to gravity loads. Available options are: <BLANK> OFFSET CONSTRAINED_OFFSET Card 1 Variable 1 ID Type I 2 3 4 5 6 7 8 HEADING A70 Card 2 1 2 3 4 5 6 7 8 Variable STRID SOILID SPR MPR Type I I Default none none I 0 I 0 VARIABLE DESCRIPTION ID Soil-structure interface ID. This is required and must be unique amongst all the contact interface IDs in the model. HEADING A descriptor for the given ID. STRID Segment set ID of base of structure at soil-structure interface. SOILID Segment set ID of soil at soil-structure interface. VARIABLE SPR DESCRIPTION Include the slave side in the *DATABASE_NCFORC and the *DATABASE_BINARY_INTFOR interface force files: EQ.1: slave side forces included. MPR Include the master side in the *DATABASE_NCFORC and the *DATABASE_BINARY_INTFOR interface force files: EQ.1: master side forces included. Remarks: See *INTERFACE_SSI_ID. The ID used for a particular interface in the static analysis must also be used for the same interface identified using *INTERFACE_SSI_ID during dynamic analysis. *INTERFACE_WELDLINE_DEVELOPMENT Purpose: This keyword causes LS-DYNA to run a weld line development calculation instead of a finite element calculation. The input for this feature consists of (1) the formed blank from a completed metal forming simulation, (2) the corresponding initial blank, and (3) if the desired weld curve on the formed blank is provided, the *INTER- FACE_WELDLINE_DEVELOPMENT method creates a weld curve on the initial blank; if the initial weld curve on the initial blank is provided, this method creates a weld curve on the final blank. Outputs also include nodes of any element edges that intersect the weld curve on the initial (affectednd_i.ibo) and final blanks (affectednd_f.ibo). Three additional keywords must be used together (and exclusively) with this keyword. They are: *INITIAL_BLANK, *FINAL_PART, and *WELDING_CURVE. NOTE: When this card is present LS-DYNA does not proceed to the finite element simulation. Card set for *INTERFACE_WELDLINE_DEVELOPMENT. Development Parameter Card. Card 1 1 2 3 4 5 6 7 8 Variable IOPTION Type Default I 1 Initial Blank Card. Following keyword *INITIAL_BLANK: Card 2 1 2 3 4 5 6 7 8 Variable Type Default FILENAME1 A80 none Final Part Card. Following keyword *FINAL_PART: Card 3 1 2 3 4 5 6 7 8 Variable Type Default FILENAME2 A80 none Welding Curve Card. Following keyword *WELDING_CURVE: Card 4 1 2 3 4 5 6 7 8 Variable Type Default FILENAME3 A80 none VARIABLE DESCRIPTION IOPTION Welding curve development options: EQ.1: Calculate initial weld curve from final (given) weld curve, with output file name weldline.ibo, which will be on the initial blank mesh. EQ.-1: Calculate final weld curve from initial weld curve, with output file name weldline_f.ibo, which will be on the formed blank mesh. FILENAME1 Initial blank file name in keyword format. FILENAME2 Final formed blank file name in keyword format. FILENAME3 File name of the weld curve, when IOPTION: EQ.1: Final (target) welding curve file name; the curve is defined using *DEFINE_CURVE_TRIM_3D. EQ.-1: Initial weld curve file name; the curve is defined using *DEFINE_CURVE_TRIM_3D. General Remarks: For metal forming of tailor welded blanks, an initial straight weld line could become a curve on the formed part. The amounts of deviation of the formed weld curve from its initial line depend on the part shape and forming conditions. Sometimes the formed weld curve is not desirable; so a correction to the initial weld curve is needed. Or, given an initial welding curve, without performing another simulation, what would the final weld curve be like? This keyword addresses these concerns. Mesh with adaptivity for the initial blank and final part is supported. Final (formed) Weld Curve: The final formed weld curve should be projected onto the final blank mesh if it does not exactly lie on the mesh surface. This can be done with LS-PrePost4.2 via the menu option GeoTol → Project → Project, select Closest Projection, select Project to Elements, then define the destination mesh and source curves, and hit Apply. Sometimes the target curve may need enough points before projection; the points may be added via menu option Curve → Spline → Method (Respace) → by number. To write the curve out in *DE- FINE_CURVE_TRIM_3D (To DE- FINE_CURVE_TRIM) → To Key, then write out the keyword using FILE → Save Keyword. format, use Curve → Convert → Method Computed Weld Curve (and IGES): Computed weld curves are written with *DEFINE_CURVE_TRIM_3D keyword into a file called weldline.ibo (or, weldline_f.ibo, depending on the IOPTION). The format of this file follows the keyword’s specification. LS-PrePost4.0 can convert the computed curve under *INTERFACE_BLANKSIZE_DEVELOPMENT. After hitting Apply, the curves will show up in the graphics window, and File → Save as → Save Geom as can be used to write the curves out in IGES format. procedures manual pages IGES, see in to Example: As shown in Figure 25-41, given the initial (initialblank.k) and final blank (finalblank.k) configuration and a final formed weld curve (finalweldingcurve.k), the following input calculates a new initial weld curve on the initial blank. In this case, the final weld curve is specified as straight in the drawn panel. *KEYWORD *INTERFACE_WELDLINE_DEVELOPMENT $OPTION 1 *INITIAL_BLANK *FINAL_PART finalblank.k *WELDING_CURVE finalweldingcurve.k *END *INTERFACE_WELDLINE_DEVELOPMENT The output is the initial weld curve in the file weldline.ibo, Figure 25-41. Nodes of element edges that intersect the initial weld curve are output in affectednd_i.ibo; while nodes of element edges that intersect the final formed weld curve are output in affectednd_f.ibo, Figure 25-42. To verify the predicted weld curve, initial blank can be re-meshed according to the curve. A draw simulation can be performed again to confirm the final weld curve as straight, Figure 25-43. Likewise, if given an initial weld curve (initialweldingcurve.k) and a final weld curve (weldline_f.ibo) can be calculated with the keyword inputs below: *KEYWORD *INTERFACE_WELDLINE_DEVELOPMENT $OPTION -1 *INITIAL_BLANK initialblank.k *FINAL_PART finalblank.k *WELDING_CURVE initialweldingcurve.k *END Final desired weld curve (input: file name under *WELDING_CURVE) Predicted initial weld curve (output: weldline.ibo) Final part (input: file name under *FINAL_PART) Initial blank (input: file name under *INITIAL_BLANK) NUMISHEET'05 Cross member Figure 25-41. An example for a welding curve development. Weld line Sheet blank mesh Figure 25-42. Nodes (in green) of element edges that intersect the weld curve are output in affectednd_i.ibo and affectednd_f.ibo, for initial and deformed mesh, respectively. Remesh initial blank according to weldline.ibo) Final weld curve confirms as straight Remeshed initial blank Final drawn part Figure 25-43. Verification run Revision information: 1. IOPTION of “1”: Revision 105189 in both double precision versions of SMP and MPP. 2. IOPTION of “-1”: Revision 105727. 3. Output of nodes of element edges that intersect the weld curve: Revision 105727. 4. Later revisions may include improvements. *KEYWORD_{OPTION} {memory} {memory2 = j} {NCPU = n} Available options include: <BLANK> ID JOBID Purpose: The keyword, *KEYWORD, flags LS-DYNA that the input deck is a keyword deck rather than the structured format, which has a strictly defined format. This must be the first card in the input file. Alternatively, by typing “keyword” on the execution line, keyword input formats are assumed and this beginning “*KEYWORD” line is not required. There are 3 optional parameters that can be specified on the *KEYWORD line. If a number {memory} is specified, it defines the memory size in units of words to be allocated. For MPP, if the parameter {memory2 = j} is given, it defines the memory allocation for rest of the MPP ranks. Note that if the memory size is specified on the execution line, it will override the memory size specified on the *KEYWORD line. If the parameter {NCPU = n} is specified it defines the number of CPUs “n” to be used during the analysis. This only applies to the Shared Memory Parallel (SMP) version of LS-DYNA. For the Distributed Memory Version (MPP), the number of CPUs is always defined with the “mpirun” command. Defining the number of CPUs on the execution line overrides what is specified on the *KEYWORD line and both override the number of CPUs specified by *CONTROL_PARALLEL. An example of the {memory} and {NCPU = n} options would be as follows: *KEYWORD 12000000 NCPU=2 This *KEYWORD command is requesting 12 million words of memory and 2 CPUs to be used for the analysis with the consistency flag turned off. To run with the consistency flag turned on (recommended), set NCPU to a negative value, e.g., “NCPU = -2” runs with 2 CPUs with the consistency flag turned on. The ID and JOBID command line options are available to add a prefix to all output and scratch file names, i.e., not the input filenames. This allows multiple simulations in a directory since a different prefix prevents files from being overwritten. If the ID option characters. ID Card. Additional Card if the ID option is active. Card 1 1 2 3 4 5 6 7 8 Variable PROJECT Type A NUM A Default none none STAGE A none VARIABLE DESCRIPTION PROJECT First part of the output file name prefix. NUM Second part of the output file name prefix. STAGE Third part of the output file name prefix. By using the ID option of *KEYWORD, an output file name prefix may be specified as a combination of the variables PROJECT, NUM and STAGE as defined on Card 1 above. For example, if these variables were set literally to “PROJECT”, “NUM”, and “STAGE”, the first d3plot would be named: PROJECT_NUM_STAGE.d3plot Alternatively, an output file name prefix can be assigned by including “jobid=” on the execution line. For example, lsdyna i=input.k jobid=PROJECT_NUM_STAGE A third way to define an output file name prefix is by using the JOBID option of the *KEYWORD command, in which case Card 1 is defined as shown below and the variable JBID acts as the output prefix. JOBID Card. Additional card if the JOBID option is active. Card 1 1 2 3 4 5 6 7 8 *KEYWORD Variable Type Default JBID A none The keyword *LOAD provides a way of defining applied forces. The keyword control cards in this section are defined in alphabetical order: *LOAD_ALE_CONVECTION_{OPTION} *LOAD_BEAM_OPTION *LOAD_BLAST *LOAD_BLAST_ENHANCED *LOAD_BLAST_SEGMENT *LOAD_BLAST_SEGMENT_SET *LOAD_BODY_OPTION *LOAD_BODY_GENERALIZED *LOAD_BODY_POROUS *LOAD_BRODE *LOAD_DENSITY_DEPTH *LOAD_ERODING_PART_SET *LOAD_GRAVITY_PART *LOAD_HEAT_CONTROLLER *LOAD_HEAT_GENERATION_OPTION *LOAD_MASK *LOAD_MOTION_NODE *LOAD_MOVING_PRESSURE *LOAD_NODE_OPTION *LOAD_REMOVE_PART *LOAD_RIGID_BODY *LOAD_SEGMENT_{OPTION} *LOAD_SEGMENT_FILE *LOAD_SEGMENT_FSILNK *LOAD_SEGMENT_NONUNIFORM_{OPTION} *LOAD_SEGMENT_SET_{OPTION} *LOAD_SEGMENT_SET_ANGLE *LOAD_SEGMENT_SET_NONUNIFORM_{OPTION} *LOAD_SEISMIC_SSI_OPTION1_{OPTION2} *LOAD_SHELL_{OPTION1}_{OPTION2} *LOAD_SPCFORC *LOAD_SSA *LOAD_STEADY_STATE_ROLLING *LOAD_STIFFEN_PART *LOAD_SUPERPLASTIC_FORMING *LOAD_SURFACE_STRESS_OPTION *LOAD_THERMAL_OPTION *LOAD_THERMAL_CONSTANT *LOAD_THERMAL_CONSTANT_ELEMENT *LOAD_THERMAL_CONSTANT_NODE *LOAD_THERMAL_D3PLOT *LOAD_THERMAL_LOAD_CURVE *LOAD_THERMAL_TOPAZ *LOAD_THERMAL_VARIABLE *LOAD_THERMAL_VARIABLE_BEAM_{OPTION} *LOAD_THERMAL_VARIABLE_ELEMENT_{OPTION} *LOAD_THERMAL_VARIABLE_NODE *LOAD_THERMAL_VARIABLE_SHELL_{OPTION} *LOAD_VOLUME_LOSS *LOAD *LOAD_ALE_CONVECTION_{OPTION} Purpose: This card is used to define the convection thermal energy transfer from a hot ALE fluid to the surrounding Lagrangian structure (remark 1). It is associated with a corresponding coupling card defining the interaction between the ALE fluid and the Lagrangian structure. It is only used when thermal energy transfer from the ALE fluid to the surrounding Lagrangian structure is significant. This is designed specifically for airbag deployment application where the heat transfer from the inflator gas to the inflator compartment can significantly affect the inflation potential of the inflator. Available options include: <BLANK> ID To define an ID number for each convection heat transfer computation in an optional card preceding all other cards for this command. This ID number can be used to output the part temperature and temperature change as functions of time in the *DATABASE_- FSI card. To do this, set the CONVID parameter in the *DATABASE_FSI card equal to this ID. ID Card. Additional card for ID keyword option. Card 1 Variable 1 ID Type I Default none 2 3 4 5 6 7 8 TITLE A70 none Include as many cards as necessary. This input terminates at the next keyword (“*”) card. Card 2 1 2 3 Variable LAGPID LAGT LAGCP Type I F F 4 H F 5 6 7 8 LAGMAS F Default none none none none none VARIABLE LAGPID DESCRIPTION Lagrangian PID (slave PID) from a corresponding coupling card which receives the thermal energy in the convection heat transfer. LAGT Initial temperature of this Lagrangian slave part. LAGCP H Constant-pressure heat capacity of this Lagrangian slave part. It has a per-mass unit (for example, J/[Kg*K]). Convection heat transfer coefficient on this Lagrangian slave part surface. It is the amount of energy (J) transferred per unit area, per time, and per temperature difference. For example, its units may be J/[m2*s*K] LAGMAS The mass of the Lagrangian slave part receiving the thermal energy. This is in absolute mass unit (for example, Kg). Remarks: 1. The only application of this card so far has been for the transfer of thermal energy from the ALE hot inflator gas to the surrounding Lagrangian structure (inflator canister and airbag-containing compartment) in an airbag deployment model. 2. The heat transferred is taken out of the inflator gas thermal energy thus reducing its inflating potential. 3. This is not a precise heat transfer modeling attempt. It is simply one mecha- nism for taking out excessive energy from the inflating potential of the hot inflator gas. 4. The heat transfer formulation may roughly be represented as following. Some representative units are shown just for clarity. [𝑄̇] = [H × 𝐴 × Δ𝑇] = ( [E] [𝐿]2[t][T] ) × [L]2 × [T] = [Power] [𝑄̇] = [𝑀̇ 𝐶𝑝(𝑇Lag New − 𝑇Lag Orig)] = ( [M] [𝑡] ) × ( [E] [M][T] ) × [T] = [E] [t] Available options include: ELEMENT SET *LOAD_BEAM Purpose: Apply the distributed traction load along any local axis of beam or a set of beams. The local axes are defined in Figure 27-1, see also *ELEMENT_BEAM. Beam Cards. Include as many as necessary. This input stops at the next keyword (“*”) card. 5 6 7 8 Card 1 2 3 Variable EID/ESID DAL LCID Type I I I 4 SF F Default none none none 1. VARIABLE EID/ESID DESCRIPTION Beam ID (EID) or beam set ID (ESID), see *ELEMENT_BEAM or *SET_BEAM. DAL = 2. The load, as shown, along the negative s-axis is produced by a positive load curve with positive scale factor (SF). n1 n2 Figure 27-1. Applied traction loads are given in force per unit length. The s and t directions are defined on the *ELEMENT_BEAM keyword. DESCRIPTION DAL Direction of applied load: EQ.1: parallel to r-axis of beam, EQ.2: parallel to s-axis of beam, EQ.3: parallel to t-axis of beam. *LOAD Load curve ID or function ID . Load curve scale factor. This is for a simple modification of the function values of the load curve. LCID SF Remark: 1.The function defined by LCID has 7 arguments: time, the 3 current coordinates, and the 3 reference coordinates. For example, using *DEFINE_FUNCTION, f(t,x,y,z,x0,y0,z0)= -10.*sqrt ( (x-x0)*(x-x0)+(y-y0)*(y-y0)+(z-z0)*(z-z0) ). applies a force proportional to the distance from the initial coordinates. *LOAD_BLAST Purpose: Define an airblast function for the application of pressure loads from the detonation of conventional explosives. The implementation is based on a report by Randers-Pehrson and Bannister [1997] where it is mentioned that this model is adequate for use in engineering studies of vehicle responses due to the blast from land mines. This option determines the pressure values when used in conjunction with the keywords: *LOAD_SEGMENT, *LOAD_SEGMENT_SET, or *LOAD_SHELL. Card 1 1 2 3 4 5 6 7 8 Variable WGT XBO YBO ZBO TBO IUNIT ISURF I 2 6 I 2 7 8 Type F F F F F Default none 0.0 0.0 0.0 0.0 Card 2 1 2 3 4 5 Variable CFM CFL CFT CFP DEATH Type F F F F F Default 0.0 0.0 0.0 0.0 0.0 VARIABLE DESCRIPTION WGT Equivalent mass of TNT. XBO YBO ZBO TBO x-coordinate of point of explosion. y-coordinate of point of explosion. z-coordinate of point of explosion. Time-zero of explosion. DESCRIPTION IUNIT Unit conversion flag. *LOAD EQ.1: feet, pound-mass, seconds, psi EQ.2: meters, kilograms, seconds, Pascals (default) EQ.3: inch, dozens of slugs, seconds, psi EQ.4: centimeters, grams, microseconds, Megabars EQ.5: user conversions will be supplied ISURF Type of burst. EQ.1: surface burst - is located on or very near the ground surface EQ.2: air burst - spherical charge (default) CFM Conversion factor - pounds per LS-DYNA mass unit. CFL CFT CFP Conversion factor - feet per LS-DYNA length units. Conversion factor - milliseconds per LS-DYNA time unit. Conversion factor - psi per LS-DYNA pressure unit DEATH Death time. Blast pressures are deactivated at this time. Remarks: 1. A minimum of two load curves, even if unreferenced, must be present in the model. 2. Segment normals should point away from the structure and nominally toward the charge. 3. Several methods can be used to approximate the equivalent mass of TNT for a given explosive. The simplest involves scaling the mass by the ratio of the Chapman-Jouguet detonation velocities given the by relationship. 𝑀TNT = 𝑀 𝐷𝐶𝐽2 𝐷𝐶𝐽TNT where MTNT is the equivalent TNT mass and DCJTNT is the Chapman-Jouguet detonation velocity of TNT. M and DCJ are, respectively, the mass and C-J velocity of the explosive under consideration. “Standard” TNT is considered to be cast with a density of 1.57 gm/cm3 and DCJTNT = 0.693 cm/microsecond. scaled distance 4. The empirical equations underlying the spherical air burst are valid for the range of (0.147 m/kg1/3 < Z < 40 m/kg1/3) where Z = R/M1/3, R is the distance from the charge center to the target and M is the TNT equivalent mass of the charge.. The range of applicability for the hemispherical surface burst is 0.45 ft/lbm1/3 < Z < 100 ft/lbm1/3 (0.178 m/kg1/3 < Z < 40 m/kg1/3). ft/lbm1/3 < Z < 100 ft/lbm1/3 0.37 5. When a charge is located on or very near the the ground surface it is considered to be a surface burst. Under this circumstance the initial blast wave is immedi- ately reflected and reinforced by the nearly unyielding ground to produce a reflected wave that moves out hemispherically from the point of burst. This reflected wave merged with the initial incident wave produces overpressures which are greater than those produced by the initial wave alone. In LS-DYNA this wave moves out spherically from the burst point so no distinction of the ground orientation is made. Target points equidistant from the burst point are loaded identically with the surface burst option. *LOAD Purpose: Define an airblast function for the application of pressure loads due the detonation of a conventional explosive. While similar to *LOAD_BLAST this feature includes enhancements for treating ground-reflected waves, moving warheads and multiple blast sources. The loads are applied to facets defined with the keyword *LOAD_BLAST_SEGMENT. A database containing blast pressure history is also available . Card Sets. Include as many sets of the following cards as necessary. This input terminates at the next keyword (“*”) card. Card 1 1 Variable BID Type I 2 M F 3 4 5 6 7 8 XBO YBO ZBO TBO UNIT BLAST F F F F Default none 0.0 0.0 0.0 0.0 0.0 Remarks Card 2 1 1 2 3 4 5 3 6 I 2 4 7 I 2 7 8 Variable CFM CFL CFT CFP NIDBO DEATH NEGPHS Type F F F F I F Default 0.0 0.0 0.0 0.0 none 1.e+20 I 0 VARIABLE DESCRIPTION BID M XBO Blast ID. A unique number must be defined for each blast source (charge). Multiple charges may be defined, however, interaction of the waves in air is not considered. Equivalent mass of TNT . x-coordinate of charge center. *LOAD_BLAST_ENHANCED DESCRIPTION YBO ZBO TBO y-coordinate of charge center. z-coordinate of charge center. Time of detonation. See Remark 3. UNIT Unit conversion flag. See Remark 4. EQ.1: pound-mass, foot,second, psi EQ.2: kilogram, meter,second, Pascal (default) EQ.3: dozen slugs (i.e., lbf-s2/in), inch, second, psi EQ.4: centimeters, grams, microseconds, Megabars EQ.5: user conversions will be supplied EQ.6: kilogram, millimeter, millisecond, GPa EQ.7: metric ton, millimeter, second, MPa EQ.8: gram, millimeter, millisecond, MPa BLAST Type of blast source. EQ.1: hemispherical surface burst – charge is located on or very near the ground surface EQ.2: spherical air burst (default) – no amplification of the initial shock wave due to interaction with the ground surface EQ.3: air burst – moving non-spherical warhead EQ.4: air burst with ground reflection – initial shock wave impinges on the ground surface and is reinforced by the reflected wave to produce a Mach front . CFM Conversion factor - pounds per LS-DYNA mass unit. CFL CFT CFP NIDBO Conversion factor - feet per LS-DYNA length units. Conversion factor - milliseconds per LS-DYNA time unit. Conversion factor - psi per LS-DYNA pressure unit. Optional node ID representing the charge center. If non-zero then XBO, YBO and XBO are ignored. DEATH Death time. Blast pressures are deactivated at this time. VARIABLE DESCRIPTION NEGPHS Treatment of negative phase. EQ.0: negative phase dictated by the Friedlander equation. EQ.1: negative phase ignored as in ConWep. Moving non-spherical warhead Card. Additional Card for BLAST = 3. Card 3 1 2 3 4 5 6 7 8 Variable VEL TEMP RATIO VID Type F F F F Default 0.0 70.0 1.0 none VARIABLE DESCRIPTION VEL Speed of warhead. TEMP Ambient air temperature, Fahrenheit. RATIO Aspect ratio of the non- spheroidal blast front. This is the longitudinal axis radius divided by the lateral axis radius. Shaped charge and EFP warheads typically have significant lateral blast resembling an oblate spheroid with RATIO < 1. Cylindrically cased explosives produce more blast in the longitudinal direction so RATIO > 1, rendering a prolate spheroid blast front, is more appropriate.. VID Vector ID representing the longitudinal axis of the warhead . This vector is parallel to the velocity vector when a non-zero velocity VEL is defined. Spherical air burst with ground reflect Card. Additional card for BLAST = 4. Card 3 1 2 3 4 5 6 7 8 Variable GNID GVID Type I I Default none none VARIABLE DESCRIPTION ID of node residing on the ground surface. ID of vector representing the vertically upward direction, i.e., normal to the ground surface . GNID GVID Remarks: 1. Several methods can be used to approximate the equivalent mass of TNT for a given explosive. The simplest involves scaling the mass by the ratio of the Chapman-Jouguet detonation velocities given the by relationship. 𝑀TNT = 𝑀 𝐷𝐶𝐽2 𝐷𝐶𝐽TNT where MTNT is the equivalent TNT mass and DCJTNT is the Chapman-Jouguet detonation velocity of TNT. M and DCJ are, respectively, the mass and C-J velocity of the explosive under consideration. “Standard” TNT is considered to be cast with a density of 1.57 gm/cm3 and DCJTNT = 0.693 cm/microsecond. 2. Segment normals should point away from the structure and nominally toward the charge unless it is the analyst’s intent to apply pressure to the leeward side of a structure. The angle of incidence is zero when the segment normal points directly at the charge. Only incident pressure is applied to a segment when the angle of incidence is greater than 90 degrees. 3. The blast time offset TBO can be used to adjust the detonation time of the charge relative to the start time of the LS-DYNA simulation. The detonation time is delayed when TBO is positive. More commonly, TBO is set negative so that the detonation occurs before time-zero of the LS-DYNA calculation. In this manner, computation time is not wasted while “waiting” for the blast wave to reach the structure. The following message, written to the messag and d3hsp files as well as the screen, is useful in setting TBO. Blast wave reaches structure at 2.7832E-01 milliseconds As an example, one might run LS-DYNA for one integration cycle and record the arrival time listed in the message above. Then TBO is set to a negative number slightly smaller in magnitude than the reported arrival time, for exam- ple TBO = -0.275 milliseconds. Under this circumstance the blast wave would reach the structure shortly after the start of the simulation. 4. Computation of blast pressure relies on an underlying method which uses base units of lbm-foot-millisecond-psi; note that this internal unit system is incon- sistent. Calculations require that the system of units in which the LS-DYNA model is constructed must be converted to this internal set of units. Predefined and user-defined unit conversion factors are available and these unit conversion factors are echoed back in the d3hsp file. Below is an example of user-defined (UNIT = 5) conversion factors for the gm-mm- millisecond-Mpa unit system. 1 = [ CFM × lb LS-DYNA mass unit 1 = [ CFL × ft LS-DYNA length unit ] = [ 2.2 × 10−3 ⏟⏟⏟⏟⏟ = CFM lbm gm ] = [3.28 × 10−3 ft mm ] ] 1 = [ CFT × ms LS-DYNA time unit ] = [1.0 ms ms ] 1 = [ CFP × psi LS-DYNA pressure unit ] = [145.0 psi MPa ] scaled distance 5. The empirical equations underlying the spherical air burst are valid for the (0.147 range of m/kg1/3 < Z < 40 m/kg1/3) where Z = R/M1/3, R is the distance from the charge center to the target and M is the TNT equivalent mass of the charge. The range of applicability for the hemispherical surface burst is 0.45 ft/lbm1/3 < Z < 100 ft/lbm1/3 (0.178 m/kg1/3 < Z < 40 m/kg1/3). ft/lbm1/3 < Z < 100 ft/lbm1/3 0.37 6. Blast loads can be used in 2D axisymmetric analyses. Repeat the second node for the third and fourth nodes of the segment definition in *LOAD_BLAST_- SEGMENT and *LOAD_BLAST_SEGMENT_SET. 7. When a charge is located on or very near the the ground surface it is considered to be a surface burst. Under this circumstance the initial blast wave is immedi- ately reflected and reinforced by the nearly unyielding ground to produce a reflected hemispherical wave that moves out from the point of burst. This reflected wave merged with the initial incident wave produces overpressures which are greater than those produced by the initial wave alone. In LS-DYNA this wave moves out spherically from the burst point so no distinction of the ground orientation is made. Target points equidistant from the burst point are loaded identically with the surface burst option. 8. The empirical equations underlying the spherical air burst with ground reflection (BLAST = 4) are valid for the range of scaled height of burst 1.0 ft/lbm1/3 < Hc//M1/3 < 7.0 ft/lbm1/3 (0.397 m/kg1/3 < Z < 2.78 m/kg1/3) where Hc is the height of the charge center above the ground and M is the TNT equiv- alent mass of the charge. F 1. *LOAD_BLAST_SEGMENT *LOAD_BLAST_SEGMENT *LOAD Purpose: Apply blast pressure loading over a triangular or quadrilateral segment for 3D geometry or line segment for 2D geometry . Segment Cards. Include as many cards as necessary. This input ends at the next keyword (“*”) card. Card 1 1 Variable BID Type I 2 N1 I 3 N2 I 4 N3 I 5 6 7 8 N4 ALEPID SFNRB SCALEP I I F Default none none none none none none 0. VARIABLE DESCRIPTION BID Blast source ID . N1 N2 N3 N4 ALEPID SFNRB Node ID. Node ID. Node ID. For line segments on two-dimensional geometries set N3 = N2. Node ID. For line segments on two-dimensional geometries set N4 = N3 = N2 or for triangular segments in three diemensions set N4 = N3. Part ID of ALE ambient part underlying this segment to be loaded by this blast . This applies only when the blast load is coupled to an ALE air domain. Scale factor for the ambient element non-reflecting boundary condition. Shocks waves reflected back to the ambient elements can be attenuated with this feature. A value of 1.0 works well for most situations. The feature is disabled when a value of zero is specified SCALEP Pressure scale factor. *LOAD_BLAST_SEGMENT_SET Purpose: Apply blast pressure loading over each segment in a segment set . Segment Set Cards. Include as many cards as necessary. This input ends at the next keyword (“*”) card. Card 1 1 2 3 4 5 6 7 8 Variable BID SSID ALEPID SFNRB SCALEP Type I I I F Default none none none 0. F 1. VARIABLE DESCRIPTION BID SSID ALEPID SFNRB Blast source ID . Segment set ID . Part ID of ALE ambient part underlying this segment to be loaded by this blast . This applies only when the blast load is coupled to an ALE air domain. Scale factor for the ambient element non-reflecting boundary condition. Shocks waves reflected back to the ambient elements can be attenuated with this feature. A value of 1.0 works well for most situations. SCALEP Pressure scale factor. Remarks: 1. Triangular segments are defined by setting N4 = N3. 2. Line segments for two-dimensional geometries are defined by setting N4 = N3 = N2. Available options include for base accelerations: *LOAD X Y Z for angular velocities: RX RY RZ for loading in any direction, specified by vector components: VECTOR and to specify a part set: PARTS Purpose: Define body force loads due to a prescribed base acceleration or angular velocity using global axes directions. This option applies nodal forces only: it cannot be used to prescribe translational or rotational motion. These body forces do not take into account non-physical mass added via mass scaling; see *CONTROL_TIMESTEP. NOTE: This data applies to all nodes in the complete prob- lem unless a part subset is specified via the *LOAD_BODY_PARTS keyword. If a part subset with *LOAD_BODY_PARTS then all nodal points belonging to the subset will have body forces applied. NOTE: Only one *LOAD_BODY_PARTS card is permitted per deck. To specify, for instance, one body load on one part and another body load on another part use *LOAD_BODY_GENERALIZED instead. For options X, Y, Z, RX, RY, RZ and VECTOR. Card 1 1 Variable LCID Type I 2 SF F Default none 1. 3 4 LCIDDR XC I 0 F 0. 8 5 YC F 0. 6 ZC F 0. 7 CID I 0 For option PARTS. Card 1 1 2 3 4 5 6 7 8 Variable PSID Type I Default none For option VECTOR. Card 2 Variable 1 V1 Type F 2 V2 F 3 V3 F Default 0.0 0.0 0.0 4 5 6 7 8 VARIABLE DESCRIPTION LCID Load curve ID, see *DEFINE_CURVE. SF Load curve scale factor LCIDDR XC YC ZC CID *LOAD DESCRIPTION Load curve ID for dynamic relaxation phase (optional). This is needed when dynamic relaxation is defined and a different load curve to LCID is required during the dynamic relaxation phase. Note if LCID is undefined then no body load will be applied during dynamic relaxation regardless of the value LCIDDR. See *CONTROL_DYNAMIC_RELAXATION 𝑥-center of rotation, define for angular velocities. 𝑦-center of rotation, define for angular velocities. 𝑧-center of rotation, define for angular velocities. Coordinate system ID to define acceleration in local coordinate system. The accelerations (LCID) are with respect to CID. EQ.0: global PSID Part set ID. V1, V2, V3 Vector components of vector 𝐕. General remarks: Translational base accelerations allow body force loads to be imposed on a structure. Conceptually, base acceleration may be thought of as accelerating the coordinate system in the direction specified, and, thus, the inertial loads acting on the model are of opposite sign. For example, if a cylinder were fixed to the 𝑦-𝑧 plane and extended in the positive x-direction, then a positive 𝑥-direction base acceleration would tend to shorten the cylinder, i.e., create forces acting in the negative 𝑥-direction. Base accelerations are frequently used to impose gravitational loads during dynamic relaxation to initialize the stresses and displacements. During the analysis, in this latter case, the body forces loads are held constant to simulate gravitational loads. When imposing loads during dynamic relaxation, it is recommended that the load curve slowly ramp up to avoid the excitation of a high frequency response. Body force loads due to the angular velocity about an axis are calculated with respect to the deformed configuration and act radially outward from the axis of rotation. Torsional effects which arise from changes in angular velocity are neglected with this option. The angular velocity is assumed to have the units of radians per unit time. The body force density is given at a point 𝐏 of the body by: (0.0,0.0,0.0) (0.0,0.0,0.0) Initial configuration Gravity-loaded shape Figure 27-2. A validation example for option VECTOR. 𝐛 = 𝜌[𝛚 × (𝛚 × 𝐫)] where 𝜌 is the mass density, 𝛚 is the angular velocity vector, and 𝐫 is a position vector from the origin to point 𝐏. Although the angular velocity may vary with time, the effects of angular acceleration are not included. Angular velocities are useful for studying transient deformation of spinning three- dimensional objects. Typical applications have included stress initialization during dynamic relaxation where the initial rotational velocities are assigned at the completion of the initialization, and this option ceases to be active. $$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ $ $$$$ *LOAD_BODY_Z $ $$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ $ $ Add gravity such that it acts in the negative Z-direction. $ Use units of mm/ms2. Since gravity is constant, the load $ curve is set as a constant equal to 1. If the simulation $ is to exceed 1000 ms, then the load curve needs to be $ extended. $ $$$ Note: Positive body load acts in the negative direction. $ *LOAD_BODY_Z $ $...>....1....>....2....>....3....>....4....>....5....>....6....>....7....>....8 $ lcid sf lciddr xc yc zc 5 0.00981 $ $ *DEFINE_CURVE $ lcid sidr scla sclo offa offo 5 $ $ abscissa ordinate 0.00 1.000 1000.00 1.000 $ $$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ About option VECTOR: The vector V defines the direction of the body force. Body forces act in the negative direction of the vector V. In an example shown in Figure 27-2, a rectangular sheet metal blank is loaded with gravity into a ball defined as a fixed rigid body. Given the global coordinate system shown, if the part set ID of the blank is 1, the keywords responsible for specifying the body force (in units of mm, second, tonne and Newton) in positive direction of (1.0, 1.0, 1.0) will be as follows, *LOAD_BODY_PARTS 1 *LOAD_BODY_VECTOR 101, 9810.0 -1.0, -1.0, -1.0 *DEFINE_CURVE 101 0.0, 1.0 10.0, 1.0 It is note that straight lines represent a cube with each edge length of 500.0mm. Revision information: The_VECTOR option is available in LS-DYNA R5 Revision 59290 and later releases. *LOAD_BODY_GENERALIZED_OPTION Available options include: SET_NODE SET_PART Purpose: Define body force loads due to a prescribed base acceleration or a prescribed angular motion over a subset of the complete problem. The subset is defined by using nodes or parts. Warning: Nodes, which belong to rigid bodies, should not be specified. Rigid bodies must be included within the part sets definitions. The body forces defined using this command do not take into account non-physical mass added via mass scaling; see *CONTROL_TIMESTEP. Card Sets. Include as many sets of Cards 1 and 2 as necessary. This input terminates at the next keyword (“*”) card. Card 1 1 2 3 4 5 Variable N1/SID N2/0 LCID DRLCID XC Type I I I Default none none none I 0 F 0. 8 6 YC F 0. 7 ZC F 0. Remarks Card 2 Variable 1 AX Type F Default 0. 2 AY F 0. 3 AZ F 0. 4 5 6 7 8 OMX OMY OMZ CID ANGTYP F 0. F 0. F 0. I 0 A CENT Remarks 1, 2 1, 2 1, 2 3, 4, 5 3, 4, 5 3, 4, 5 optional VARIABLE DESCRIPTION N1/SID Beginning node ID for body force load or the node or part set ID. N2 Ending node ID for body force load. Set to zero if a set ID is defined. LCID Load curve ID, see *DEFINE_CURVE. DRLCID Load curve ID for dynamic relaxation phase. Only necessary if dynamic relaxation is defined. See *CONTROL_DYNAMIC_RE- LAXATION. XC YC ZC AX AY AZ OMX OMY OMZ CID 𝑥-center of rotation. Define only for angular motion. 𝑦-center of rotation. Define only for angular motion. 𝑧-center of rotation. Define only for angular motion. Scale factor for acceleration in 𝑥-direction Scale factor for acceleration in 𝑦-direction Scale factor for acceleration in 𝑧-direction Scale factor for 𝑥-angular velocity or acceleration Scale factor for 𝑦-angular velocity or acceleration Scale factor for 𝑧-angular velocity or acceleration Coordinate system ID to define acceleration local coordinate system. The coordinate (XC, YC, ZC) is defined with respect to the local coordinate system if CID is nonzero. The accelerations, LCID and their scale factors are with respect to CID. in the EQ.0: global *LOAD_BODY_GENERALIZED DESCRIPTION ANGTYP Type of body loads due to angular motion EQ.CENT: body load from centrifugal acceleration, 𝜌[𝛚 × (𝛚 × 𝐫)]. EQ.CORI: body load from Coriolis-type acceleration, EQ.ROTA: body load from rotational acceleration, 2𝜌(𝛚 × 𝐯). 𝜌(𝛂 × 𝐫), where 𝛚 is the angular velocity, 𝛂 is the angular acceleration, 𝐫 is the position vector relative to cen- ter of rotation and 𝐯 is the velocity vector Remarks: 1. Translational base accelerations allow body forces loads to be imposed on a structure. Conceptually, base acceleration may be thought of as accelerating the coordinate system in the direction specified, and, thus, the inertial loads acting on the model are of opposite sign. For example, if a cylinder were fixed to the y-z plane and extended in the positive x-direction, then a positive x-direction base acceleration would tend to shorten the cylinder, i.e., create forces acting in the negative x-direction. 2. Base accelerations are frequently used to impose gravitational loads during dynamic relaxation to initialize the stresses and displacements. During the analysis, in this latter case, the body forces loads are held constant to simulate gravitational loads. When imposing loads during dynamic relaxation, it is recommended that the load curve slowly ramp up to avoid the excitation of a high frequency response. 3. Body force loads due to the angular motion about an axis are calculated with respect to the deformed configuration. When ANGYP = CENT or CORI, tor- sional effects which arise from changes in angular velocity are neglected. Such torsional effects can be taken into account by setting ANGTYP = ROTA. The angular velocity is assumed to have the units of radians per unit time, accord- ingly angular acceleration has the units of radians/time2. 4. The body force density is given at a point 𝐏 of the body by: 𝒃 = 𝜌[𝛚 × (𝛚 × 𝐫)] where 𝜌 is the mass density, 𝛚 is the angular velocity vector, and 𝐫 is a position vector from the origin to point 𝐏. Although the angular velocity may vary with time, the effects of angular acceleration are included. 5. Angular velocities are useful for studying transient deformation of spinning three-dimensional objects. Typical applications have included stress initializa- tion during dynamic relaxation where the initial rotational velocities are as- signed at the completion of the initialization, and this option ceases to be active. *LOAD_BODY_POROUS Purpose: Define the effects of porosity on the flow with body-force-like loads applied to the ALE element nodes. Ergun porous flow assumptions are used. This only applies to non-deformable (constant-porosity), fully saturated porous media. This model only works with a non-zero and constant viscosity fluid defined via either *MAT_NULL or *MAT_ALE_VISCOUS card. Card Sets. Include as many sets of Cards 1 and 2 as necessary. This input terminates at the next keyword (“*”) card. 3 AX F 4 AY F 5 AZ F 6 BX F 7 BY F 8 BZ F 0.0 0.0 0.0 0.0 0.0 0.0 3 4 5 6 7 8 Card 1 1 2 Variable SID SIDTYP I 0 2 Type Default I 0 Card 2 1 Variable AOPT Type Default I 0 VARIABLE DESCRIPTION SID Set ID of the ALE fluid part subjected to porous flow condition. SIDTYP Set ID type of the SID above. If SIDTYP = 0 (default), then the SID = PSID (part set ID). If SIDTYP = 1, then SID = PID (part ID). AX, AY, AZ Viscous coefficients for viscous terms in global 𝑥, 𝑦, and 𝑧 directions (please see equation below). If 𝐴𝑥 ≠ 0 and 𝐴𝑦 = 𝐴𝑧 = 0 then an isotropic viscous permeability condition is assumed for the porous medium. VARIABLE BX, BY, BZ DESCRIPTION Inertial coefficients for inertia terms in global 𝑥, 𝑦, and 𝑧 directions (please see equation below). If 𝐵𝑥 ≠ 0, and 𝐵𝑦 = 𝐵𝑧 = 0 then an isotropic inertial permeability condition is assumed for the porous medium. AOPT Material axis option: EQ.0: inactive. EQ.1: The forces are applied in a local system attached to the ALE solid . Remarks: 1. Consider the basic general Ergun equation for porous flow in one direction: Δ𝑃 Δ𝐿 = 𝑘1 𝑉𝑠 + 𝑘2 2 𝑉𝑠 Where 𝜌 = Fluid Density 𝜇 = Fluid dynamic vicosity 𝑉𝑠 = 4𝑄 𝜋𝐷2 = Superficial fluid velocity 𝑄 = Overall volume flow rate ( m3 ) 𝐷 = Porous channel characteristic width (perpendicular to ΔL) 𝜀3𝑑𝑝 𝑘1 = 150(1 − 𝜀)2 = Permeability parameter 𝑘2 = 𝜀3𝑑𝑝 1.75(1 − 𝜀) = Passability parameter 𝜖 = Porosity= total pore volume total media volume 𝑑𝑝 = Effective particle diameter 2. The above equation can be generalized into 3 dimensional flows where each component may be written as − 𝑑𝑃 𝑑𝑥𝑖 = 𝐴𝑖𝜇𝑉𝑖 + 𝐵𝑖𝜌|𝑉𝑖|𝑉𝑖 where 𝑖 = 1,2,3 refers to the global coordinate directions (no summation intend- ed for repeated indices), 𝜇 is the constant dynamic viscosity, 𝜌 is the fluid densi- ty, 𝑉𝑖 is the fluid velocity components, 𝐴𝑖 is analogous to 𝑘1 above, and 𝐵𝑖 is analogous to 𝑘2 above. A matrix version can be defined by ALE elements with *DEFINE_POROUS_ALE. 3. If 𝐵𝑖 = 0, the equation is reduced to simple Darcy Law for porous flow (may be good for sand-like flow). For coarse grain (rocks) media, the inertia term will be important and the user needs to input these coefficients. *LOAD Purpose: Define Brode function for application of pressure loads due to explosion, see Brode [1970], also see *LOAD_SEGMENT, *LOAD_SEGMENT_SET, or *LOAD_SHELL. Card 1 1 2 3 4 5 6 7 8 Variable YLD BHT XBO YBO ZBO TBO TALC SFLC Type F F F F F F Default 0.0 0.0 0.0 0.0 0.0 0.0 Remarks Card 2 1 2 3 4 5 6 I 0 1 7 I 0 1 8 Variable CFL CFT CFP Type F F F Default 0.0 0.0 0.0 VARIABLE DESCRIPTION YLD BHT XBO YBO ZBO TBO TALC Yield (Kt, equivalent tons of TNT). Height of burst. x-coordinates of Brode origin. y-coordinates of Brode origin. z-coordinates of Brode origin. Time offset of Brode origin. Load curve number giving time of arrival versus range relative to Brode origin (space, time), see *DEFINE_CURVE and remark below. Load curve number giving yield scaling versus scaled time (time relative to Brode origin divided by [yield(**1⁄3)]) origin (space, time), see *DEFINE_CURVE and remark below. Conversion factor - kft to LS-DYNA length units. Conversion factor - milliseconds to LS-DYNA time units. Conversion factor - psi to LS-DYNA pressure units. *LOAD VARIABLE SFLC CFL CFT CFP Remarks: 1. If these curves are defined a variable yield is assumed. Both load curves must be specified for the variable yield option. If this option is used, the shock time of arrival is found from the time of arrival curve. The yield used in the Brode formulas is computed by taking the value from the yield scaling curve at the current time/[yield(**1⁄3)] and multiplying that value by yield. *LOAD Purpose: Define density versus depth for gravity loading. This option has been occasionally used for analyzing underground and submerged structures where the gravitational preload is important. The purpose of this option is to initialize the hydrostatic pressure field at the integration points in the element. This card should be only defined once in the input deck. Card 1 1 Variable PSID Type Default I 0 Remarks 1,2 2 GC F 0.0 3 4 5 6 7 8 DIR LCID I 1 I none 3 VARIABLE DESCRIPTION PSID GC DIR Part set ID, see *SET_PART. If a PSID of zero is defined then all parts are initialized. Gravitational acceleration value. Direction of loading: EQ.1: global x, EQ.2: global y, EQ.3: global z. LCID Load curve ID defining density versus depth, see *DEFINE_- CURVE. Remarks: 1. Density versus depth curves are used to initialize hydrostatic pressure due to gravity acting on an overburden material. The hydrostatic pressure acting at a material point at depth, d, is given by: 𝑑surface 𝑝 = − ∫ 𝜌(𝑧)𝑔𝑑𝑧 where 𝑝 is pressure, 𝑑surface, is the depth of the surface of the material to be initialized (usually zero), 𝜌 (𝑧) is the mass density at depth 𝑧, and 𝑔 is the accel- eration of gravity. This integral is evaluated for each integration point. Depth may be measured along any of the global coordinate axes, and the sign conven- tion of the global coordinate system should be respected. The sign convention of gravity also follows that of the global coordinate system. For example, if the positive 𝑧 axis points "up", then gravitational acceleration should be input as a negative number. 2. For this option there is a limit of 12 parts that can be defined by PSID, unless all parts are initialized. 3. Depth is the ordinate of the curve and is input as a descending x, y, or z coordinate value. Density is the abscissa of the curve and must vary (increase) with depth, i.e., an infinite slope is not allowed. 4. See also GRAV in *PART. *LOAD Purpose: Apply a pressure load to the exposed surface composed of solid elements that may erode. Card Sets. Include as many sets of Cards 1 and 2 as necessary. This input terminates at the next keyword (“*”) card. Card Variable 1 ID 2 LCID Type I I Default none none Card 2 1 Variable IFLAG Type Default I 0 2 X F 5 6 7 8 PSID BOXID MEM ALPHA I 0 6 I F 50 80 7 8 3 SF F 1 3 Y F 4 AT F I 0.0 none 4 Z F 5 BETA F 0.0 0.0 0.0 90 VARIABLE DESCRIPTION ID LCID SF AT ID number. Load curve ID defining pressure as a function of time, see *DE- FINE_CURVE. Scale factor. Arrival time. PSID Part set ID, see *SET_PART. BOXID Box ID, see *DEFINE_BOX. Any segment that would otherwise be loaded but whose centroid falls outside of this box is not loaded. MEM ALPHA IFLAG *LOAD_ERODING_PART_SET DESCRIPTION Extra memory, in percent, to be allocated above the initial memory for storing the new load segments exposed by the erosion. The maximum angle (in degrees) permitted between the normal of a segment at its centroid and the average normal at its nodes. This angle is used to eliminate interior segments. Flag for choosing a subset of the exposed surface that is oriented towards a blast or other loading source. The vector from the center of the element to the source location must be within an angle of BETA of the surface normal. If IFLAG > 0, then the subset is chosen, otherwise if IFLAG = 0, the entire surface is loaded. X, Y, Z Optional source location. BETA Maximum permitted angle (in degrees) between the surface normal and the vector to the source. The exposed segment is not loaded if the calculated angle is greater than BETA. Remarks: 1. 2. If LCID is input as -1, then the Brode function is used to determine the pressure for the segments, see *LOAD_BRODE. If LCID is input as -2, then an empirical air blast function is used to determine the pressure for the segments, see *LOAD_BLAST. 3. The load curve multipliers may be used to increase or decrease the pressure. The time value is not scaled. 4. The activation time, AT, is the time during the solution that the pressure begins to act. Until this time, the pressure is ignored. The function value of the load curves will be evaluated at the offset time given by the difference of the solu- tion time and AT i.e., (solution time-AT). 5. For proper evolution of the loaded surface, it is a requirement that DTMIN in *CONTROL_TERMINATION be greater trhan zero and ERODE in *CON- TROL_TIMESTEP be set to 1. Available options are: <BLANK> SET *LOAD Purpose: Define gravity for individual parts. This feature is intended for use with *LOAD_STIFFEN_PART to simulate staged construction. This keyword is available for solids and shells, and also beam element types 1, 2, 6, and 9. It is not currently available for thick shells. Part Cards. Include this card as many times as necessary. This input ends at the next keyword (“*”) card. Card 1 1 2 Variable PID DOF Type I I 3 LC I Default none none none 4 5 6 7 8 ACCEL LCDR STGA STGR F 0 I none I 0 I 0 DESCRIPTION VARIABLE PID/PSID DOF LC Part ID (or Part Set ID for the_SET option) for application of gravity load Direction: enter 1, 2 or 3 for 𝑥, 𝑦 or 𝑧 Load curve defining factor vs. time (or zero if STGA, STGR are defined) ACCEL Acceleration (will be multiplied by factor from curve Load curve defining factor vs. time during dynamic relaxation Construction stage at which part is added (optional) Construction stage at which part is removed (optional) LCDR STGA STGR Remarks: 1. There are 3 options for defining how the gravity load on a part varies with time. a) Curve LC gives factor vs time. This overrides the other methods if LC is non-zero. b) STGA, STGR refer to stages at which part is added and removed – the stages are defined in *DEFINE_CONSTRUCTION_STAGES. If STGA is zero, the gravity load starts at time zero. If not, it ramps up from the small factor FACT (on *CONTROL_STAGED_CONSTRUCTION) up to full val- ue over the ramp time at the start of stage STGA. If STGR is zero, the gravity load continues until the end of the analysis. If not, it ramps down from full value to FACT over the ramp time at the start of stage STGR. c) *DEFINE_STAGED_CONSTRUCTION_PART can be used instead of *LOAD_GRAVITY_PART to define this loading. During initialization, a LOAD_GRAVITY_PART card will be created and the effect is the same as using the STGA, STGR method described above; ACCEL is then taken from *CONTROL_STAGED_CONSTRUCTION. 2. This feature calculates the loading from the mass of the elements of the referenced parts only (density × volume). This mass does not include any at- tached lumped mass elements. Only solid, beam and shell elements can be loaded. *LOAD Purpose: Used to define a thermostat control function. The thermostat controls the heat generation within a material by monitoring a remote nodal temperature. Control can be specified as on-off, proportional, integral, or proportional with integral. Sensor Node Cards. Include up to 20 cards. This input ends at the next keyword (“*”) card. Card 1 1 2 3 4 5 Variable NODE PID LOAD TSET TYPE Type I I F F I 8 6 GP F 7 GI F Default none none none none none none none VARIABLE DESCRIPTION NODE Sensor is located at this node number. PID LOAD TSET Part ID assigned to the elements modeling the heater or cooler being controlled. Heater output 𝑞0. [typical units: W/m3] Controller set point temperature at the location identified by NODE. TYPE Type of control function. EQ.1: on-off EQ.2: proportional + integral GP GI Proportional gain. Integral gain. Remarks: The thermostat control function is 𝑞 ̇′′′ = 𝑞 ̇0 ′′′ [𝐺𝑃(𝑇set − 𝑇node) + 𝐺𝐼 ∫ (𝑇set − 𝑇node) 𝑑𝑡] 𝑡=0 *LOAD_HEAT_GENERATION_OPTION Available options include: SOLID SET_SOLID SHELL SET_SHELL Purpose: Define elements or element sets with heat generation. Generation Cards. Include as many cards as necessary. This input ends at the next keyword (“*”) card. Card 1 1 2 3 4 5 6 7 8 Variable SID LCID MULT WBLCID CBLCID TBLCID Type I I F Default none none 0. I 0 I 0 I 0 VARIABLE DESCRIPTION SID LCID Element ID or element set ID, see *ELEMENT_SOLID, *SET_SOL- ID, *ELEMENT_SHELL, and *SET_SHELL, respectively. Volumetric heat generation rate, 𝑞 ̇′′′, specification. SI units are W/m3. This parameter can reference a load curve ID or a function ID . When the reference is to a curve, LCID has the following interpretation: GT.0: 𝑞 ̇′′′ is defined by a curve consisting of (time, 𝑞 ̇′′′) data pairs. EQ.0: 𝑞 ̇′′′ is a constant defined by the value MULT. LT.0: 𝑞 ̇′′′ is defined by a curve consisting of (temperature, 𝑞 ̇′′′) data pairs. Enter |-LCID| on the DEFINE_CURVE keyword. MULT Volumetric heat generation, 𝑞̇′′′, curve multiplier. DESCRIPTION Load curve ID defining the blood perfusion rate [e.g., kg/m3 sec] as a function of time. Load curve ID defining the blood specific heat [e.g., J/kg C] as a function of the blood temperature. Load curve ID defining the blood temperature [e.g., C] as a function of time. VARIABLE WBLCID CBLCID TBLCID Remarks: 1. If LCID references a DEFINE_FUNCTION, the following function arguments are allowed 𝑓 (𝑥, 𝑦, 𝑧, 𝑣𝑥, 𝑣𝑦, 𝑣𝑧, 𝑇, 𝑡)where: 𝑥, 𝑦, 𝑧 = element centroid coordinates 𝑣𝑥, 𝑣𝑦, 𝑣𝑧 = element centroid velocity components 𝑇 = element integration point temperature 𝑡 = solution time 2. Rate of heat transfer from blood to tissue = 𝑊𝑏𝐶𝑏(𝑇𝑏 − 𝑇) [units: J/m3 sec] *LOAD_MASK Purpose: Apply a distributed pressure load over a three-dimensional shell part. The pressure is applied to a subset of elements that are within a fixed global box and lie either outside or inside of a closed curve in space which is projected onto the surface. Card Sets. Include as many sets of Cards 1 and 2 as necessary. This input terminates at the next keyword (“*”) card. Card 1 1 2 3 4 5 6 7 8 Variable PID LCID VID1 OFF BOXID LCIDM VID2 INOUT Type I I F Default none none 1. F 0. I 0 I 0 I none I 0 4 5 6 7 8 Remarks 1 Card 2 1 2 Variable ICYCLE 2 3 Type I Default 200 Remarks VARIABLE DESCRIPTION PID LCID Part ID (PID). This part must consist of 3D shell elements. To use this option with solid element the surface of the solid elements must be covered with null shells. See *MAT_NULL. Curve ID defining the pressure time history, see *DEFINE_- CURVE. VID1 OFF BOXID LCIDM VID2 INOUT ICYCLE *LOAD DESCRIPTION Vector ID normal to the surface on which the applied pressure acts. Positive pressure acts in a direction that is in the opposite direction. This vector may be used if the surface on which the pressure acts is relatively flat. If zero, the pressure load depends on the orientation of the shell elements as shown in Figure 27-4. Pressure loads will be discontinued if ∣𝑉𝐼𝐷1 ⋅ 𝑛𝑠ℎ𝑒𝑙𝑙∣ < 𝑂𝐹𝐹 where 𝑛𝑠ℎ𝑒𝑙𝑙 is the normal vector to the shell element. Only elements inside the box with part ID, PID, are considered. If no ID is given all elements of part ID, PID, are included. When the active list of elements are updated, elements outside the box the current will no configuration is always used. longer have pressure applied, i.e., Curve ID defining the mask. This curve gives (x,y) pairs of points in a local coordinate system defined by the vector ID, VID2. Generally, the curve should form a closed loop, i.e., the first point is identical to the last point, and the curve should be flagged as a DATTYP = 1 curve in the *DEFINE_CURVE section. If no curve ID is given, all elements of part ID, PID, are included with the exception of those deleted by the box. The mask works like the and trimming option, Figure15-18. see DEFINE_CURVE_TRIM i.e., Vector ID used to project the masking curve onto the surface of part ID, PID. The origin of this vector determines the origin of the local system that the coordinates of the PID are transformed into prior to determining the pressure distribution in the local system. This curve must be defined if LCIDM is nonzero. See Figure15-18. If 0, elements whose center falls inside the projected curve are considered. If 1, elements whose center falls outside the projected curve are considered. Number of time steps between updating the list of active elements (default = 200). The list update can be quite expensive and should be done at a reasonable interval. The default is not be appropriate for all problems. 1. The part ID must consist of 3D shell elements. *LOAD_MASK *LOAD Purpose: Apply a concentrated nodal force or moment to a node based on the motion of another node. Node Cards. This input continues until the next keyword (“*”) card. Card 1 2 3 Variable NODE1 DOF1 LCID Type I I I 4 SF F Default none none none 1. Remarks 5 6 7 8 CID1 NODE2 DOF2 CID2 I 0 1 I 0 I 0 I 0 1 VARIABLE DESCRIPTION NODE1 Node ID for the concentrated force. DOF1 Applicable degrees-of-freedom: EQ.1: x-direction of load action, EQ.2: y-direction of load action, EQ.3: z-direction of load action, EQ.4: moment about the x-axis, EQ.5: moment about the y-axis, EQ.6: moment about the z-axis. LCID SF CID1 Load curve ID or function ID . The applied force is a function of the applicable degree-of-freedom of NODE2. Load curve scale factor. Coordinate system ID (optional), see remark 1 on next page. NODE2 Node ID for calculating the force. *LOAD_MOTION_NODE DESCRIPTION DOF2 Applicable degrees-of-freedom: EQ.1: x-coordinate EQ.2: y-coordinate, EQ.3: z-coordinate, EQ.4: x-translational displacement, EQ.5: y-translational displacement, EQ.6: z-translational displacement, EQ.7: rotational displacement about the x-axis, EQ.8: rotational displacement about the y-axis, EQ.9: rotational displacement about the z-axis. EQ.10: x-translational velocity, EQ.11: y-translational velocity, EQ.12: z-translational velocity, EQ.13: rotational velocity about the x-axis, EQ.14: rotational velocity about the y-axis, EQ.15: rotational velocity about the z-axis. CID2 Coordinate system ID (optional), see Remark 1. Remarks: 1. The global coordinate system is the default. The local coordinate system ID’s are defined in the *DEFINE_COORDINATE_SYSTEM section. *LOAD Purpose: Apply moving pressure loads to a nondisjoint surface. The pressure loads approximate a jet of high velocity fluid impinging on the surface. Multiple surfaces may be defined each acted on by a set of nozzles. Card 1 1 2 3 4 5 6 7 8 Variable LOADID Type I Default none Nozzle Cards. Define the following cards for each nozzle. Include as many cards as desired. This input ends at the first card with the second field (NODE2) <= 3. Card 2 1 2 3 4 5 6 7 8 Variable NODE1 NODE2 LCID CUTOFF LCIDT LCIDD Type I I I F Default none none none none I 0 I 0 The following card defines the surface where the nozzles act. Card 3 Variable 1 ID 2 3 4 5 6 7 8 IDTYPE NIP Type I I I Default none none 3x3 VARIABLE DESCRIPTION LOADID Loading ID. NODE1 Node located at the origin of the nozzle. *LOAD_MOVING_PRESSURE DESCRIPTION NODE2 Node located at the head of the nozzle LCID CUTOFF LCIDT LCIDD ID IDT Load curve or function ID defining pressure versus radial distance from the center of the jet. Outer radius of jet. The pressure acting outside this radius is set to zero. Load curve or function ID, which scales the pressure as a function of time. If a load curve isn’t specified, the scale factor defaults to 1.0. Load curve or function ID, which scales the pressure as a function of distance from the nozzle. If a load curve isn’t specified, the scale factor defaults to 1.0. Segment set ID, shell element set ID, part set ID, or part ID. See IDT below. Slave segment or node set type. The type must correlate with the number specified for SSID: EQ.0: segment set ID for surface-to-surface contact, EQ.1: shell element set ID for surface-to-surface contact, EQ.2: part set ID, EQ.3: part ID, NIP Number of integration in segment used to compute pressure loads. Available options include: POINT SET *LOAD Purpose: Apply a concentrated nodal force to a node or each node in a set of nodes. Node/Node set Cards. Include as many cards as necessary. This input ends at the next keyword (“*”) card. Card 1 2 3 Variable NID/NSID DOF LCID Type I I I 4 SF F Default none none none 1. Remarks 7 M2 I 0 8 M3 I 0 5 CID I 0 1 6 M1 I 0 2 VARIABLE DESCRIPTION NID/NSID Node ID or nodal set ID (NSID), see *SET_NODE_OPTION. DOF Applicable degrees-of-freedom: EQ.1: 𝑥-direction of load action, EQ.2: 𝑦-direction of load action, EQ.3: 𝑧-direction of load action, EQ.4: follower force , EQ.5: moment about the 𝑥-axis , EQ.6: moment about the 𝑦-axis axis , EQ.7: moment about the 𝑧-axis axis , EQ.8: follower moment . LCID Load curve ID or function ID . m1 m3m3 m2 Figure 27-3. Nodes M1, M2, and M3 define a plane. A positive follower force acts in the positive 𝑡-direction of that plane, i.e., along the normal vector of the plane. A positive follower moment puts a counterclockwise torque about the normal vector. The normal vector is found by the cross product 𝐭 = 𝐯 × 𝐰 where 𝐯 and 𝐰 are vectors as shown. VARIABLE DESCRIPTION Load curve scale factor. Coordinate system ID (optional), see Remark 1 on next page. Node 1 ID. Only necessary if DOF.EQ.4 or 8, see Remark 2 below. Node 2 ID. Only necessary if DOF.EQ.4 or 8, see Remark 2 below. Node 3 ID. Only necessary if DOF.EQ.4 or 8, see Remark 2 below. SF CID M1 M2 M3 Remarks: 1. Coordinate Systems. The global coordinate system is the default. The local coordinate system ID’s are defined in the *DEFINE_COORDINATE_SYSTEM section. 2. Follower Forces. The current position of nodes 𝑀1, 𝑀2, 𝑀3 are used to control the direction of a follower force. A positive follower force acts normal to the plane defined by these nodes, and a positive follower moment puts a counter- clockwise torque about the 𝑡-axis. These actions are depicted in Figure 27-3. An alternative way to define the force direction is by setting 𝑀3 to any non- positive value, in which case the follower force is in the 𝑀1 𝑡𝑜 𝑀2 direction. 3. Axisymmetric Elements with Area and Volume Weighting. For shell formulations 14 and 15, the axisymmetric solid elements with area and volume weighting, respectively, the specified nodal load is per unit length (type14) and per radian (type 15). 4. Moments. Moments can only be applied to nodes that have rotational degrees of freedom. Element type and formulation determine the degrees of freedom for a node, e.g., the nodes of solid formulation 1 have only 3 translational de- grees of freedom and no rotational degrees of freedom. 5. *DEFINE_FUNCTION for LCID. The function defined by LCID has 7 arguments: time, the 3 current coordinates, and the 3 reference coordinates. A function that applies a force proportional to the distance from the initial coordi- nates would be: f(t,x,y,z,x0,y0,z0)= -10.*sqrt ( (x-x0)*(x-x0)+(y-y0)*(y-y0)+(z-z0)*(z-z0) ) $$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ $ $$$$ *LOAD_NODE_SET $ $$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ $ $ A cantilever beam (made from shells) is loaded on the two end nodes $ (nodes 21 & 22). The load is applied in the y-direction (dof=2). $ Load curve number 1 defines the load, but is scaled by sf=0.5 in the $ *LOAD_NODE_SET definition. $ *LOAD_NODE_SET $ $...>....1....>....2....>....3....>....4....>....5....>....6....>....7....>....8 $ nsid dof lcid sf cid m1 m2 m3 14 2 1 0.5 $ $ *SET_NODE_LIST $ sid 14 $ $ nid1 nid2 nid3 nid4 nid5 nid6 nid7 nid8 21 22 $ $ *DEFINE_CURVE $ lcid sidr scla sclo offa offo 1 $ $ abscissa ordinate 0.0 0.0 10.0 100.0 20.0 0.0 $ $ $$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ Available options include: <BLANK> SET *LOAD_REMOVE_PART Purpose: Delete the elements of a part in a staged construction simulation. Shock effects are prevented by gradually reducing the stresses prior to deletion. Available only for solid and shell elements. Note: This keyword card will be available starting in release 3 of version 971. Part Cards. Include as many cards as necessary. This input ends at the next keyword (“*”) card. Card 1 1 2 3 4 5 6 7 8 Variable PID/PSID TIME0 TIME1 STGR Type I Default none F 0 F 0 I 0 VARIABLE DESCRIPTION PID Part ID (or Part Set ID for the_SET option) for deletion Time at which stress reduction starts Time at which stresses become zero and elements are deleted Construction stage at which part is removed (optional) TIME0 TIME1 STGR Remarks: There are 3 methods of defining the part removal time: 1. TIME0, TIME1 override all the other methods if non-zero 2. STGR refers to the stage at which the part is removed – the stages are defined in *DEFINE_CONSTRUCTION_STAGES. This is equivalent to setting TIME0 and TIME1 equal to the start and end of the ramp time at the beginning of stage STGR. 3. *DEFINE_STAGED_CONSTRUCTION_PART can be used instead of *LOAD_- REMOVE_PART to define this loading. During initialization, a STIFFEN_- PART card will be created and the effect is the same as using the STGA, STGR method described above. *LOAD_RIGID_BODY Purpose: Apply a concentrated nodal force to a rigid body. The force is applied at the center of mass or a moment is applied around a global axis. As an option, local axes can be defined for force or moment directions. Rigid Body Cards. Include as many Rigid Body Cards as necessary. This input ends at the next keyword (“*”) card. Card 1 1 2 3 Variable PID DOF LCID Type I I I 4 SF F Default none none none 1. Remark 7 M2 I 0 8 M3 I 0 5 CID I 0 1 6 M1 I 0 2 VARIABLE DESCRIPTION PID DOF Part ID of the rigid body, see *PART_OPTION. Applicable degrees-of-freedom: EQ.1: x-direction of load action, EQ.2: y-direction of load action, EQ.3: z-direction of load action, EQ.4: follower force, see Remark 2, EQ.5: moment about the x-axis, EQ.6: moment about the y-axis, EQ.7: moment about the z-axis. EQ.8: follower moment, see Remark 2. LCID Load curve ID or function ID . GT.0: force as a function of time, LT.0: force as a function of the absolute value of the rigid body displacement. This option only applies to load curves. VARIABLE DESCRIPTION Load curve scale factor Coordinate system ID Node 1 ID. Only necessary if DOF.EQ.4 or 8, see Remark 2. Node 2 ID. Only necessary if DOF.EQ.4 or 8, see Remark 2. Node 3 ID. Only necessary if DOF.EQ.4 or 8, see Remark 2. SF CID M1 M2 M3 Remarks: 1. The global coordinate system is the default. The local coordinate system ID’s are defined in the *DEFINE_COORDINATE_SYSTEM section. This local axis is fixed in inertial space, i.e., it does not move with the rigid body. 2. Nodes M1, M2, M3 must be defined for a follower force or moment. The follower force acts normal to the plane defined by these nodes as depicted in Figure 27-3. The positive t-direction is found by the cross product 𝑡 = 𝑣 × 𝑤 where v and w are vectors as shown. The follower force is applied at the center of mass. A positive follower moment puts a counterclockwise torque about the t-axis. 3. When LCID defines a function, the function has seven arguments: time, the 3 current coordinates for the center of mass, and the 3 reference coordinates. A function that applies a force proportional to the distance from the initial coordi- nates would be f(t,x,y,z,x0,y0,z0)= -10.*sqrt ( (x-x0)*(x-x0)+(y-y0)*(y-y0)+(z-z0)*(z-z0) ). $$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ $ $$$$ *LOAD_RIGID_BODY $ $$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ $ $ From a sheet metal forming example. A blank is hit by a punch, a binder is $ used to hold the blank on its sides. The rigid holder (part 27) is held $ against the blank using a load applied to the cg of the holder. $ $ The direction of the load is in the y-direction (dof=2) but is scaled $ by sf = -1 so that the load is in the correct direction. The load $ is defined by load curve 12. $ *LOAD_RIGID_BODY $ $...>....1....>....2....>....3....>....4....>....5....>....6....>....7....>....8 $ pid dof lcid sf cid m1 m2 m3 27 2 12 -1.0 $ $ *DEFINE_CURVE $ lcid sidr scla sclo offa offo 12 $ $ abscissa ordinate 0.000E+00 8.000E-05 1.000E+04 8.000E-05 $ $$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ *LOAD To define an ID for the segment loading, the following option is available: ID If the ID is defined an additional card is required. Purpose: Apply the distributed pressure load over one triangular or quadrilateral segment defined by four, six, or eight nodes, or in the case of two-dimensional geometries, over one two-noded line segment. The pressure and node numbering convention follows the Figure 27-4 shown in the remarks below. ID Card. Additional card for the ID keyword option. Card 1 Variable 1 ID Type I 2 3 4 5 6 7 8 HEADING A70 Card 2 1 Variable LCID Type I 2 SF F 3 AT F 4 N1 I 5 N2 I 6 N3 I 7 N4 I 8 N5 I Default none 1. 0. none none none none none Remarks 1 2 3 4,5,6,7 n 3 s n 6 n 5 n 1 n 4 n 2 n 4 n 8 n 1 t n 7 n 5 n 3 n 6 n Figure 27-4. Nodal numbering for pressure segments in three-dimensional geometries. Positive pressure acts in the negative t-direction. 4 5 6 7 8 Addition card for when N5 ≠ 0. Card 3 Variable 1 N6 Type I 2 N7 I 3 N8 I Default none none none VARIABLE DESCRIPTION ID Loading ID HEADING A description of the loading. LCID Load curve ID or function ID . SF Load curve scale factor VARIABLE DESCRIPTION Arrival time for pressure or birth time of pressure. Node ID Node ID Node ID Node ID. Repeat N3 for 3-node triangular segments. Mid-side node ID, if applicable . Mid-side node ID, if applicable . Mid-side node ID, if applicable . Mid-side node ID, if applicable . AT N1 N2 N3 N4 N5 N6 N7 N8 Remarks: 1. If LCID is input as -1, then the Brode function is used to determine the pressure for the segments, see *LOAD_BRODE. If LCID is input as -2, then an empirical airblast function is used to determine the pressure for the segments, see *LOAD_BLAST. 2. The load curve multipliers may be used to increase or decrease the pressure. The time value is not scaled. 3. The activation time, AT, is the time during the solution that the pressure begins to act. Until this time, the pressure is ignored. The function value of the load curves will be evaluated at the offset time given by the difference of the solu- tion time and AT i.e., (solution time-AT). 4. Triangular segments without mid-side nodes are defined by setting N4 = N3. To apply a uniform pressure to type 17 tetrathedral elements, 4 triangular seg- ments should be defined for each loaded face of an element. Three of the seg- ments should each have one corner node and the two adjacent mid-side node. The 4th segment should be made from the 3 mid-side nodes. 5. To apply a uniform pressure to type 16 tetrahedral elements or type 24 type triangular shell elements, one 6 node segment may be defined for each loaded face. However, LS-DYNA will accept and properly treat “any” other segment definition. In other words, if the preprocessor happens to create one 3-noded segment corresponding to local node numbering convention {1,2,3,3} in Figure 27-4, or permutations thereof, then this will internally be detected as a 6-noded segment and the nodal forces will be consistently distributed over the 6 in- volved nodes. Likewise, if four 3-noded segments corresponding to local node numbering conventions {1,4,6,6}, {2,5,4,4}, {3,6,5,5} and {4,5,6,6}, or permuta- tions thereof, are created, then these will be detected to belong to the same 6- noded segment and again result in the correct nodal forces. The difference be- tween the two latter approaches is that using four “sub-segments” will provide four different normal directions 𝒕 instead of just one, and for curved faces this will provide a more accurate representation of the pressure load. 6. To apply a uniform pressure to type 23 hexahedral elements or type 23 quadrilateral shell elements, one 8 node segment may be defined for each load- ed face. However, LS-DYNA will accept and properly treat a segment exclud- ing the 4 mid side nodes. In other words, if the preprocessor happens to create just one 4-noded segment corresponding to local node numbering convention {1,2,3,4} in Figure 27-4, or permutations thereof, then this will internally be detected as a 8-noded segment and the nodal forces will be consistently distrib- uted over the 8 involved nodes. 7. To apply a uniform pressure to type 24 hexahedral elements, either one 4 node segment corresponding to the numbering convention {1,2,3,4} in Figure 27-4, or permutations thereof, may be defined for each loaded face. But LS-DYNA will also accept and properly treat four 4 node segments corresponding to {1,5,9,8}, {2,6,9,5}, {3,7,9,6} and {4,8,9,7}, where local node number 9 is located in the cen- ter of the face. The difference between these two approaches is that using four “sub-segments” will provide four different normal directions 𝒕 instead of just one, and for curved faces this will provide a more accurate representation of the pressure load. 8. Segments for two-dimensional geometries are defined by two nodes, N1 and N2. Leave N3 and N4 as zero or else set both equal to N2. A positive pressure acts on the segment in the Z x (N1-N2) direction where Z is the global Z-axis and (N1-N2) is the vector from N1 to N2. 9. The function defined by LCID has 7 arguments: time, the 3 current coordinates, and the 3 reference coordinates. A function that applies a pressure proportional to the distance from the initial coordinates would be: f(t,x,y,z,x0,y0,z0)= sqrt ( (x-x0)*(x-x0)+(y-y0)*(y-y0)+(z-z0)*(z-z0) ) $$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ $ $$$$ *LOAD_SEGMENT $ $$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ $ $ A block of solid elements is pressed down onto a plane as it moves along $ that plane. This pressure is defined using the *LOAD_SEGMENT keyword. $ $ The pressure is applied to the top of the block. This top is defined $ by the faces on top of the appropriate solid elements. The faces are $ defined with segments. For example, nodes 97, 106, 107 & 98 define $ a top face on one of the solids (and thus, one of the faces to apply the $ pressure too). This "face" is referred to as a single segment. $ $ The load is defined with load curve number 1. The curve starts at zero, $ ramps to 100 in 0.01 time units and then remains constant. However, $ the curve is then scaled by sclo = 2.5. Thus, raising the load to 250. $ Note that the load is NOT scaled in the *LOAD_SEGMENT keyword, but $ could be using the sf variable. $ *LOAD_SEGMENT $ $...>....1....>....2....>....3....>....4....>....5....>....6....>....7....>....8 $ lcid sf at n1 n2 n3 n4 1 1.00 0.0 97 106 107 98 1 1.00 0.0 106 115 116 107 1 1.00 0.0 98 107 108 99 1 1.00 0.0 107 116 117 108 $ $ *DEFINE_CURVE $ $ lcid sidr scla sclo offa offo 1 0 0.0 2.5 $ $ abscissa ordinate 0.000 0.0 0.010 100.0 0.020 100.0 $ $$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ *LOAD_SEGMENT_CONTACT_MASK Purpose: Mask the pressure from a *LOAD_SEGMENT_SET when the pressure segments are in contact with another material. This keyword is currently only supported in the MPP version. Note that the Heading Card is required. Heading Card. Card 1 Variable 1 ID Type I Load Set Card. Card 2 1 Variable LSID Type I 2 3 4 5 6 7 8 HEADING A70 2 P1 F 3 P2 F 4 5 6 7 8 CID1 CID2 CID3 CID4 CID5 I I I I I Optional Cards. This data ends at the next “*” card. Card 2 1 2 3 4 5 6 7 8 Variable CID6 CID7 CID8 CID9 CID10 CID11N CID12 CID13 Type I I I I I I I I VARIABLE DESCRIPTION LSID P1 Load set ID to mask, which must match a *LOAD_SEGMENT_- SET. See Remark 2. Lower pressure limit. When the surface pressure due to contact is below P1, no masking is done and the full load defined in *LOAD_SEGMENT_SET is applied. For pressures between P1 and P2 see Remark 1. VARIABLE DESCRIPTION P2 CIDn Upper pressure limit. When the surface pressure due to contact is above P2, no load is applied due to the *LOAD_SEGMENT_SET. For pressures between P1 and P2 see Remark 1. The IDs of contacts that can mask the pressure loads. The specified contact definitions must all be of the same type. Furthermore, only non-automatic SURFACE_TO_SURFACE (two way) or AUTOMATIC_SURFACE_TO_SURFACE_TIEBREAK are supported. For TIEBREAK contacts, pressure is masked until the tie fails. Once the tie fails, the full pressure will be applied for the remainder of the simulation. The values P1 and P2 are ignored. For other contact types, the contact forces, along with the nodal contact surface areas, are used to compute the contact pressure at each node to determine any masking effect. Remarks: 1. Intermediate Pressures. If the contact pressure, 𝑝contact is between P1 and P2, the pressure load is scaled by a factor of P1 may be set equal to P2 if desired. 𝑓 = P2 − 𝑝contact 𝑃2 − 𝑃1 . 2. LSID. The LSID values must be unique. Having two instances of this referencing the same*LOAD_SEGMENT_SET is not supported. However, a contact ID may appear in two different instances of this keyword. *LOAD_SEGMENT_FILE Purpose: To define time-varying distributed pressure loads over triangular or quadrilateral segments defined by four, six, or eight nodes via a binary file. Card 1 Variable Type 1 FILENAME A80 Card 2 is required but may be left blank. Card 2 1 2 3 4 5 6 7 8 Variable LCID Type I Default none VARIABLE FILENAME DESCRIPTION Filename of binary database containing segment pressures versus time. There are three sections in this database. LCID Optional Load curve ID defining segment pressure scale factor versus time. *LOAD_SEGMENT_FILE Each database is assumed to be written with a block size equal to a multiple of 512 words, with each block containing 1 or more states. If the data does not complete the last block it is padded with zeros. The code will open and read next family file if it detects phony word or EOF. If the IO returns a zero length read, the code assumes end of IO and strop reading. Linear interpolation is used if IO can find current time between two states. Therefore, the given database can have more states than simulation time steps. Linear extrapolation will only be used when IO reaches end of the database. The last two states will be used and code will issue warning message “MSG_SOL+1323” to d3hsp and messag files. Section Words Description Control Section 64 words Segment Data 4 words Mid-side Nodes 4 Words. Ommitted unless NSEG < 0. 10 1 1 1 1 1 1 1 1 1 Title NSEG: The absolute value, |"NSEG" | specifies the number of segments contained within the file. If NSEG < 0, then the file contains mid- side nodes. N1; Node ID. N2: Node ID. N3: Node ID. geometries. Repeat N2 for two-dimensional N4: Node ID. Repeat N2 for two-dimensional geometries or repeat N3 for 3-node triangular segments. N5: Optional mid-side node ID. N6: Optional mid-side node ID. N7: Optional mid-side node ID. N8: Optional mid-side node ID. ⋮ 4 or 8 ⋮ NSEGth segment data 4 or 8 Last set of segment data “State” Section 1 + |NSEG| words 1 1 ⋮ Time Segment Pressure ⋮ ⋮ 1 1 NSEG Pressure of last segment ⋮ ⋮ *LOAD Purpose: Apply distributed pressure loads from a previous ALE analysis to a specified segment set in the current analysis. This capability trades some of the model’s accuracy for a large reduction in model size. NOTE: The deck for the “previous” run must include a *DATABASE_BINARY_FSILNK card to activate the creation of the fsilink file. Either the *LOAD_SEG- MENT_FSILNK card (this card) or the *DATA- BASE_BINARY_FSILNK card may be in an input deck, but not both. Card 1 1 2 3 4 5 6 7 8 Variable Type FILENAME A80 Card 2 1 2 3 4 5 6 7 8 Variable NINT LCID Type I Default none I 0 Coupling ID Cards. Read in NINT coupling IDs. Repeat this card as many times as necessary to input all NINT values. Card 3 1 Variable ID1 2 ID2 3 ID3 4 ID4 5 ID5 6 ID6 7 ID7 8 ID8 Type I I Default none none *LOAD_SEGMENT_FSILNK DESCRIPTION FILENAME Filename of the interface linking file. NINT LCID IDi Number of couplings for which the previous run provides pressure data. Load curve ID or function ID . The curve referred to by LCID provides a scale factor as a function of time. The pressure data that is read in from the fsilnk file is scaled according to this value. These must match COUPIDs from the *CONSTRAINED_LA- GRANGE_IN_SOLID card from the previous runs. These IDs specify which of the first run’s couplings are propagated into this run through pressure data read from the fsilnk file. The algorithm: This feature provides a method for using pressure time history data from *CON- STRAINED_LAGRANGE_IN_SOLID Lagrangian-to-ALE couplings in one calculation as pressure data for the same segment in subsequent calculations. The time range covered by the subsequent calculation must overlap the time range of the initial calculation. First calculation: Write out pressure data. 1. Add a *DATABASE_BINARY_FSILNK card to the first run. 2. Specify filename for the fsilnk file by adding a command line argument to ls- dyna. ls-dyna … fsilnk=fsi_filename … Without a *DATABASE_BINARY_FSILNK card this command line argument will have no effect. Format of fsilnk File: WRITE: Job title (character*80 TITLE) WRITE: Number of interfaces (integer NINTF) For 𝑖 = 1 to NINTF { WRITE: Number of segments in the ith interface (integer NSEG[𝑖]) For 𝑗 = 1 to NSEG[𝑖] { WRITE: Connectivities of jth segment in the ith interface (integer*4) } } For 𝑛 = 1 to number of time steps { WRITE: time value for the nth time step (real) For 𝑖 = 1 to NINTF For 𝑗 = 1 to NSEG[𝑖] { WRITE: Pressure for the jth segment of the ith interface (real) } } } Subsequent calculations: Read fsilnk File. Include this keyword, *LOAD_SEGMENT_FSILNK, and be careful to remove the *DATABASE_BINARY_FSILNK keyword. Specify the name of the fsilnk file from the previous run on *LOAD_SEGMENT_FSILNK’s first data card. Then, at each time step, the pressure of the specified coupling IDs is set on the Lagrangian-mesh side from data in the fsilnk file. For times outside of the fsilnk file’s range LS-DYNA extrapolates. 1. If current time is before the 1st fsilnk time, then pressure is set to 0. 2. If the current time is in the range of times in the fsilnk file, then the pressure is linearly interpolated from the data at the two time states in the fsilnk file brack- eting the current time. 3. If the current time is after the last fsilnk time, then the pressure is set to the fsilnk pressure at last time step. *LOAD_SEGMENT_NONUNIFORM_{OPTION} To define an ID for the non-uniform segment loading the following option is available: ID If the ID is defined an additional card is required. Purpose: Apply a distributed load over one triangular or quadrilateral segment defined by three, four, six, or eight nodes. The loading and node numbering convention follows Figure 27-3. ID Card. Additional card for ID keyword option. Optional Variable 1 ID Type I 2 3 4 5 6 7 8 HEADING A70 Card Sets. Each segment is specified by a set of the following 3 cards. Include as many sets as necessary. This input ends at the next keyword (“*”) card. Card 1 1 Variable LCID Type I 2 SF F 3 AT F 4 DT F Default none 1. 0. 1.E+16 Remarks 1 2 3 3 5 CID I 0 4 6 V1 F 7 V2 F 8 V3 F none none none Card 2 Variable 1 N1 Type I 2 N2 I 3 N3 I 4 N4 I 5 N5 I 6 N6 I 7 N7 I 8 N8 I Default none none none none none none none none Card 3 Variable 1 P1 Type F 2 P2 F 3 P3 F 4 P4 F 5 P5 F 6 P6 F 7 P7 F 8 P8 F Default none none none none none none none none VARIABLE DESCRIPTION ID Loading ID HEADING A description of the loading. LCID Load curve ID or function ID . For a load curve ID the load curve must provide pressure as a function of time. For a function ID, the function is expected to have seven arguments: current time minus the birth time, the current x, y, and z coordinates, and the initial x, y, and z coordinates. LT.0: Applies to 3, 4, 6 and 8-noded segments. With this option the load becomes a follower load, meaning that the direc- tion of the load is constant with respect to the local seg- ment coordinate system. SF AT DT Load curve scale factor Arrival/birth time for the traction load. Death time for the traction load. CID Coordinate system ID V1, V2, V3 *LOAD_SEGMENT_NONUNIFORM DESCRIPTION Vector direction cosines relative to coordinate system CID defining the direction of the traction loading. Note that for LCID.LT.0 this vector rotates with the geometry of the segment. N1 N2 N3 N4 N5 N6 N7 N8 P1 P2 P3 P4 P5 P6 P7 P8 Node ID Node ID Node ID. Repeat N2 for two-dimensional geometries. Node ID. Repeat N2 for two-dimensional geometries or repeat N3 for 3-node triangular segments. Optional mid-side node ID . Optional mid-side node ID . Optional mid-side node ID . Optional mid-side node ID . Scale factor at node ID, N1. Scale factor at node ID, N2. Scale factor at node ID, N3. Scale factor at node ID, N4. Scale factor at node ID, N5. Scale factor at node ID, N6. Scale factor at node ID, N7. Scale factor at node ID, N8. *LOAD To define an ID for the segment loading, the following option is available: ID If the ID is defined an additional card is required. Purpose: Apply the distributed pressure load over each segment in a segment set. See *LOAD_SEGMENT for a description of the pressure sign convention and remarks on high order segment definitions. ID Card. Additional card for the ID keyword option. Optional Variable 1 ID Type I 2 3 4 5 6 7 8 HEADING A70 Segment Set Cards. Include as many segment set cards as necessary. This input ends at the next keyword (“*”) card. 5 6 7 8 Card 1 1 2 Variable SSID LCID Type I I 3 SF F Default none none 1. Remarks 1 2 4 AT F 0. 3 VARIABLE DESCRIPTION SSID Segment set ID, see *SET_SEGMENT. Load curve ID or function ID . For a load curve ID the load curve must provide pressure as a function of time. For a function ID the function is expected to have seven arguments: current time minus the birth time, the current x, y, and z coordinates, and the initial x, y, and z coordinates. Load curve scale factor Arrival time for pressure or birth time of pressure. *LOAD VARIABLE LCID SF AT Remarks: 1. If LCID is input as -1, then the Brode function is used to determine pressure for the segment set, also see *LOAD_BRODE. If LCID is input as -2, then an empir- ical airblast function is used to determine the pressure for the segments, see *LOAD_BLAST. 2. The load curve multipliers may be used to increase or decrease the pressure. The time value is not scaled. 3. The activation time, AT, is the time during the solution that the pressure begins to act. Until this time, the pressure is ignored. The function value of the load curves will be evaluated at the offset time given by the difference of the solu- tion time and AT i.e., (solution time-AT). *LOAD Purpose: Apply the traction load over a segment set that is dependent on the orientation of a vector. An example application is applying a pressure to a cylinder as a function of the crank angle in an automobile engine. The pressure and node numbering convention follows Figure 27-4. Card Sets. Include as many sets of Cards 1 and 2 as desired. This input ends at the next keyword (“*”) card. Card 1 Variable 1 ID 2 3 4 5 6 7 8 IDSS LCID SCALE IOPTP IOPTD I 0 5 I 0 6 7 8 Type I I I F Default none none none 1. Card 2 Variable 1 N1 Type I 2 N2 I 3 NA I 4 NI I Default none none none none VARIABLE DESCRIPTION ID IDSS LCID Loading ID Segment set ID. Load curve or function ID defining the traction as a function of the angle. If IOPT = 0 below, define the abscissa between 0 and 2π radians or 0 and 360 degrees if IOPD = 1. SCALE Scale factor on value of the load curve or function. IOPTP *LOAD_SEGMENT_SET_ANGLE DESCRIPTION Flag for periodicity. The default (IOPTP = 0) requires the load curve to be defined between 0 and 2π. This is useful, for example, for modeling an engine that is running at a steady state since each rotation will experience the same loading. To model a transient response, IOPTP = 1 uses a load curve defined over the full range of angles, permitting a different response on the second and subsequent revolutions. IOPTD Flag for specifying if the load curve or function argument is in radians (IOPTD = 0, the default) or degrees (IOPTD = 1). N1 N2 NA NI The node specifying the tail of the rotating vector. The node specifying the head of the rotating vector. The node specifying the head of the vector defining the axis of rotation. The node N1 specifies the tail. The node specifying the orientation of the vector at an angle of zero. If the initial angle is zero, NI should be equal to N2. z y x N2 initial α, angle N1 NI NA *LOAD_SEGMENT_SET_NONUNIFORM_{OPTION} To define an ID for the non-uniform segment loading the following option is available: ID If the ID is defined an additional card is required. Purpose: Apply the traction load over one triangular or quadrilateral segment defined by three or four nodes. The pressure and node numbering convention follows Figure 27-4. ID Card. Additional card for ID keyword option. Optional Variable 1 ID Type I 2 3 4 5 6 7 8 HEADING A70 Card Sets. Include as many pairs of Cards 1 and 2 as desired. This input ends at the next keyword (“*”) card. Card 1 1 2 Variable SSID LCID Type I I 3 SF F Default none none 1. Card 2 1 Variable CID Type Default I 0 2 V1 F 3 V2 F none none none 5 6 7 8 DT ELTYPE F A 1016 none 5 6 7 8 4 AT F 0. 4 V3 N4 Edge 4 N1 Edge 1 Edge 3 N3 Edge 2 N2 Figure 27-5. Local coordinates system for edge load. VARIABLE DESCRIPTION ID Loading ID HEADING A description of the loading. SSID LCID Segment set ID. Load curve ID or function ID . The seven arguments for the function are current time minus the birth time, the current x, y, and z coordinates, and the initial x, y, and z coordinates. LT.0: Applies to 3, 4, 6 and 8-noded segment sets. With this option the load becomes a follower load, meaning that the direction of the load is constant with respect to the local segment coordinate system. The local coordinate system for edge load, see ELTYPE, is shown in Fig- ure 27-5. SF AT DT Load curve scale factor Arrival/birth time for pressure. Death time for pressure. VARIABLE ELTYPE DESCRIPTION Optional edge loading type. If left blank, pressure on the segment will be applied. EQ.EF1: Distributed force per unit length along edge 1, Figure 27-5. EQ.EF2: Distributed force per unit length along edge 2, Figure 27-5. EQ.EF3: Distributed force per unit length along edge 3, Figure 27-5. EQ.EF4: Distributed force per unit length along edge 4, Figure 27-5. CID Coordinate system ID V1, V2, V3 Vector direction cosines relative to the coordinate system CID defining the direction of the traction loading. Note that for LCID.LT.0 this vector rotates with the geometry of the segment. *LOAD_SEISMIC_SSI_OPTION1_{OPTION2} Available options for OPTION1 include: NODE SET POINT OPTION2 allows an optional ID to be given: ID Purpose: Apply earthquake load due to free-field earthquake ground motion at certain locations — defined by either nodes or coordinates — on a soil-structure interface, for use in earthquake soil-structure interaction analysis. The specified motions are used to compute a set of effective forces in the soil elements adjacent to the soil-structure interface, according to the effective seismic input–domain reduction method [Bielak and Christiano (1984)]. ID Card. Additional card for the ID keyword option. Optional Variable 1 ID Type I 2 3 4 5 6 7 8 HEADING A70 Card Sets. Include as many pairs of Cards 1 and 2 as desired. This input ends at the next keyword (“*”) card. Node and set Cards. Card 1 for keyword options NODE or SET: Card 1 1 2 3 4 5 6 7 8 Variable SSID typeID GMX GMY GMZ Type I I I I I Default none none none none none Point Cards. Card 1 for keyword option POINT. Card 1 1 2 3 4 5 6 7 8 9 10 Variable SSID Type I Default none XP F 0. YP F 0. ZP F 0. GMX GMY GMZ I I I none none none Card 2 Variable 1 SF 2 3 4 5 6 7 8 CID BIRTH DEATH ISG IGM Type F Default 1. I 0 F 0. F 1028 I 0 I 0 VARIABLE DESCRIPTION ID Optional ID. This ID does not need to be unique. HEADING An optional descriptor for the given ID. SSID Soil-structure interface ID. typeID Node ID (NID in *NODE) or nodal set ID (SID in *SET_NODE). XP YP ZP GMX GMY GMZ 𝑥 coordinate of ground motion location on soil-structure interface. 𝑦 coordinate of ground motion location on soil-structure interface. 𝑧 coordinate of ground motion location on soil-structure interface. Acceleration load curve or ground motion ID for motion in the (local) 𝑥-direction. Acceleration load curve or ground motion ID for motion in the (local) 𝑦-direction. Acceleration load curve or ground motion ID for motion in the (local) 𝑧-direction. SF CID *LOAD_SEISMIC_SSI DESCRIPTION Ground motion scale factor. (default = 1.0) Coordinate system ID, see *DEFINE_COORDINATE_SYSTEM. BIRTH Time at which specified ground motion is activated. DEATH Time at which specified ground motion is removed: EQ.0.0: default set to 1028 ISG Definition of soil-structure interface: EQ.0: SSID is ID for soil-structure interface defined by *INTER- FACE_SSI_ID for non-matching mesh between soil and structure. EQ.1: SSID is segment set ID identifying soil-structure interface for merged meshes between soil and structure. IGM Specification of ground motions GMX, GMY, GMZ: EQ.0: ground motions are specified as acceleration load curves. See *DEFINE_CURVE EQ.1: Both ground accelerations and velocities specified using *DEFINE_GROUND_MOTION. Remarks: 1. The ground motion at any node on a soil-structure interface is computed as follows: a) If the node coincides with a location where ground motion is specified, that ground motion is used for that node. b) If the node does not coincide with a location where ground motion is specified, the ground motion at that node along a particular degree-of- freedom is taken as a weighted average of all the ground motions speci- fied on the interface along that degree-of-freedom, where the weights are inversely proportional to the distance of the node from the ground motion location. 2. Multiple ground motions specified at the same location are added together to obtain the resultant ground motion at that location. 3. Spatially-uniform ground motion may be specified on a soil-structure interface by specifying the ground motion at only one location on that interface. Specify- ing the ground motion at more than one point on a soil-structure interface re- sults in spatially-varying ground motion on that interface. *LOAD_SHELL_OPTION1_{OPTION2} Available options for OPTION1 include: ELEMENT SET Available options for OPTION2 include: ID If the ID is defined an additional card is required. Purpose: Apply the distributed pressure load over one shell element or shell element set. The numbering of the shell nodal connectivities must follow the right hand rule with positive pressure acting in the negative t-direction. See Figure 27-4. This option applies to the three-dimensional shell elements only. ID Card. Additional card for ID keyword option. Optional Variable 1 ID Type I 2 3 4 5 6 7 8 HEADING A70 Shell Cards. Include as many of these cards as desired. This input ends at the next keyword (“*”) card. 5 6 7 8 Card 1 1 2 Variable EID/ESID LCID Type I I 3 SF F Default none none 1. Remarks 1 1 2 4 AT F 0. EID/ESID *LOAD DESCRIPTION Shell ID (EID) or shell set ID (ESID), see *ELEMENT_SHELL or *SET_SHELL. LCID Load curve ID, see *DEFINE_CURVE. Load curve scale factor Arrival time for pressure or birth time of pressure. SF AT Remarks: 1. 2. If LCID is input as -1, then the Brode function is used to determine the pressure for the segments, see also *LOAD_BRODE. If LCID is input as -2, then the ConWep function is used to determine the pressure for the segments, see *LOAD_BLAST. 3. The load curve multipliers may be used to increase or decrease the pressure. The time value is not scaled. $$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ $ $$$$ *LOAD_SHELL_ELEMENT $ $$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ $ $ From a sheet metal forming example. A blank is hit by a punch, a holder is $ used to hold the blank on its sides. All shells on the holder are given a $ pressure boundary condition to clamp down on the blank. The pressure $ follows load curve 3, but is scaled by -1 so that it applies the load in the $ correct direction. The load starts at zero, but quickly rises to 5 MPa $ after 0.001 sec. (Units of this model are in: ton, mm, s, N, MPa, N-mm) $ *LOAD_SHELL_ELEMENT $ $...>....1....>....2....>....3....>....4....>....5....>....6....>....7....>....8 $ eid lcid sf at 30001 3 -1.00E+00 0.0 30002 3 -1.00E+00 0.0 30003 3 -1.00E+00 0.0 30004 3 -1.00E+00 0.0 30005 3 -1.00E+00 0.0 30006 3 -1.00E+00 0.0 30007 3 -1.00E+00 0.0 $ $ Note: Just a subset of all the shell elements of the holder is shown above, $ in practice this list contained 448 shell element id's. $ $ *DEFINE_CURVE $ lcid sidr scla sclo offa offo 3 $ $ abscissa ordinate 0.000 0.0 0.001 5.0 0.150 5.0 $ $ $$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ *LOAD Purpose: When used in a full-deck restart run, this card will apply the SPC constraint forces from the initial run on the corresponding degrees of freedom in the current run. This is useful when modeling unbounded domains using a non-reflecting boundary while incorporating static stresses computed in the initial run: the fixed constraints on the outer boundary in the initial static analysis are removed in the transient analysis and replaced by equivalent static forces. While *BOUNDARY_NON_REFLECTING acts similarly if dynamic relaxation is used for the static analysis, this approach works for any method used to preload the model. No parameters are necessary for this card. *LOAD_SSA Purpose: The Sub-Sea Analysis (SSA) capability allows a simple and efficient way of loading the structure to account for the effects of the primary shock wave and the subsequent bubble oscillations of an underwater explosion. It achieves its efficiency by approximating the pressure scattered by air and water-backed plates and the pressure transmitted through a water-back plate. The loading incorporates the plane wave approximation for direct shock response and the virtual mass approximation for bubble response. *LOAD_SSA does not implement a doubly asymptotic approximation of transient fluid-structure interaction. Card 1 Variable 1 VS Type F 2 DS F 3 REFL F Default none none 0. 4 ZB F 0. 5 6 7 8 ZSURF FPSID PSID NPTS F 0. I 0 I 0 I 1 Card Sets. Include as many pairs of Cards 1 and 2 as necessary. This input ends at the next keyword (“*”) card. Card 1 Variable Type 1 A F 2 3 4 5 6 7 8 ALPHA GAMMA KTHETA KAPPA F F F F Default none none none none none Card 2 Variable 1 XS Type F 2 YS F 3 ZS F 4 W F 5 6 TDELY RAD F F 7 CZ F 8 Default none none none none none none none VARIABLE DESCRIPTION VS DS Sound speed in fluid Density of fluid REFL Consider reflections from sea floor. EQ.0: off EQ.1: on ZB Z coordinate of sea floor if REFL = 1, otherwise, not used. ZSURF Z coordinate of sea surface FPSID Part set ID of parts subject to flood control. Use the *PART_SET_- COLUMN option where the parameters A1 and A2 must be defined as follows: Parameter A1: Flooding status: EQ.1.0: Fluid on both sides. EQ.2.0: Fluid outside, air inside. EQ.3.0: Air outside, fluid inside. EQ.4.0: Material or part is ignored. Parameter A2: Tubular outer diameter of beam elements. For shell elements this input must be greater than zero for loading. PSID Part set IDs of parts defining the wet surface. The elements defining these parts must have their outward normals pointing into the fluid. See Figure 27-6. EQ.0: all parts are included. GT.0: the part set id. NPTS Number of integration points for computing pressure (1 or 4) A Shock pressure parameter ALPHA α, shock pressure parameter GAMMA γ, time constant parameter Elements covering the surface must have outward facing normal vectors Figure 27-6. The shell elements interacting with the fluid must be numbered such that their outward normal vector points into the fluid media. VARIABLE DESCRIPTION KTHETA KAPPA 𝐾𝜃, time constant parameter κ, ratio of specific heat capacities XS YS ZS W X coordinate of charge Y coordinate of charge Z coordinate of charge Weight of charge TDELY Time delay before charge detonates RAD CZ Charge radius Charge depth Remarks: 1. SSA assumes the model is in MKS units. If it is in another system of units, *control_coupling should be used to account for the conversion. 2. The “flooding status” is instrumental in determining how the model parts are loaded. If A1 = 1, the front of the plate as defined by the outward normal is exposed to the incident pressure. The back of the plate is not exposed to the incident pressure but feels a transmitted pressure that resists plate motion. If A1 = 2, then the plating has fluid on the outside as determined by the outward normal. It is exposed to the incident pressure and feels the scattered pressure. No loading is applied to the back side. If A1 = 3, then air is on the front of the plate and water is on the back. Neither the front nor the back of the plate is exposed to the incident pressure, but the motion of the plate is resisted by pres- sure generated on the back of the plate when it moves. Transmitted pressures are assumed not to strike another plate. 3. The pressure history of the primary shockwave at a point in space through which a detonation wave passes is given as: 𝑃(𝑡) = 𝑃𝑚𝑒 −𝑡 𝜃 where 𝑃𝑚 and the time constant 𝜃 below are functions of the type and weight W of the explosive charge and the distance 𝑄 from the charge. 𝑃𝑝𝑒𝑎𝑘 = 𝐴 [ ] 𝑊1/3 𝜃 = 𝐾𝜃𝑊1/3 [ ] 𝑊1/3 where A, α, γ, and Κθ are constants for the explosive being used. *LOAD_STEADY_STATE_ROLLING Steady state rolling analysis is a generalization of *LOAD_BODY, allowing the user to apply body loads to part sets due to translational and rotational accelerations in a manner that is more general than the *LOAD_BODY capability. *LOAD_STEADY_- STATE_ROLLING may be invoked multiple times as long as no part has the command applied more than once. Furthermore, the command may be applied to arbitrary meshes, i.e., axisymmetric meshes are not required. Card Sets. Include as many sets consisting of the following four cards as desired. This input ends at the next keyword (“*”) card. Card 1 Variable 1 ID 2 3 4 5 6 7 8 PSID Type I I Default none none Card 2 Variable Type Default Card 3 Variable Type 4 Default 1 N1 I 0 1 N3 I 0 2 N2 I 0 2 N4 I 0 3 4 5 6 7 8 LCD1 LCD1R I 0 3 I 0 4 LCD2 LCD2R I 0 I 0 5 6 7 Card 4 Variable Type Default 1 N5 I 0 2 N6 I 0 3 4 5 6 7 8 LCD3 LCD3R I 0 I 0 VARIABLE DESCRIPTION ID PSID N1 N2 ID Part set ID Node 1 defining rotational axis Node 2 defining rotational axis LCD1 Load curve defining angular velocity around rotational axis. LCD1R Optional load curve defining angular velocity around rotational axis for dynamic relaxation. LCD1 is used during dynamic relaxation if LCD1R is not defined. N3 N4 Node 3 defining turning axis Node 4 defining turning axis LCD2 Load curve defining angular velocity around turning axis. LCD2R N5 N6 LCD3 LCD3R Optional load curve defining angular velocity around turning axis for dynamic relaxation. LCD2 is used during dynamic relaxation if LCD2R is not defined. Node 5 defining translational direction Node 6 defining translational direction Load curve defining translational velocity direction. in translational load in Optional translational direction. LCD3 is used during dynamic relaxation if LCD3R is not defined. translational velocity curve defining *LOAD_STEADY_STATE_ROLLING The steady state rolling capability adds inertial body loads in terms of a moving reference defined by the user input. The current coordinates are defined in terms of the displacement, u, and the moving reference frame, Y, 𝑥𝑆𝑆𝑅 = 𝑢 + 𝑌 𝑥̇𝑆𝑆𝑅 = 𝑢̇ + 𝑌̇ 𝑥̈𝑆𝑆𝑅 = 𝑢̈ + 𝑌̈ 𝑌 = 𝑅(𝜔2𝑡)[𝑅(𝜔1𝑡)(𝑋 − 𝑋𝑂) − 𝑋𝐶] + 𝑌𝑇(𝑡) where R is the rotation matrix obtained by integrating the appropriate angular velocity, the magnitude of the angular velocities 𝜔1 and 𝜔2 are defined by load curves LCD1 and LCD2 respectively, and the directions are defined by the current coordinates of the node pairs N1-N2 and N3-N4 . The velocity corresponding to the translational term, YT(t), is defined in magnitude by LCD3 and in direction by the node pair N5-N6. The initial coordinates of the nodes are X, XO is the initial coordinate vector of node N1 and XC is the initial coordinate vector of node N3. If data defining an angular velocity is not specified, the velocity is defaulted to zero, and R is the identity matrix. In a similar manner, if the translational velocity is not specified, it is defaulted to zero. This capability is useful for initializing the stresses and velocity of tires during dynamic relaxation, and rolling processes in manufacturing. It is available for solid formulations 1, 2, 10, 13, and 15, and for shell formulations 2, 4, 5, 6, 16, 25, 26, and 27. It is not available for beams and tshells. It is available for implicit and explicit simulations and is invoked for dynamic relaxation by specifying that the load curves are used during dynamic relaxation. At the end of the dynamic relaxation, the velocities of the parts are set to 𝑥̇𝑆𝑆𝑅and the remaining parts are initialized according to the input file. Users must ensure that the appropriate load curves are turned on during the relaxation process, and if implicit dynamic relaxation is used, that sufficient constraints are applied during the initialization to remove any rigid body motion and that they are removed at the end of the dynamic relaxation. The implicit iteration convergence rate is often improved by adding the geometric stiffness matrix using *CONTROL_IMPLIC- IT_GENERAL. A consistent tangent matrix is available by using *CONTROL_IMPLIC- IT_GENERAL, and while it improves the convergence rate with problems with small strains, it is often unstable for problems with large strains. The *CONTROL_STEADY_- STATE_ROLLING options should be used to ramp up the frictional forces to obtain smooth solutions and good convergence rates. To obtain the free-rolling angular velocity, the tire should be first inflated, then brought into contact with the road while the frictional force is ramped up with a load curve and a large value of SCL_K specified in *CONTROL_STEADY_STATE_ROLLING. The angular velocity of the tire is then slowly varied over a range that covers the free rolling velocity. The free rolling velocity is obtained when either the frictional force in the direction of rolling or the moment about the tire axis is near zero. For a tire with an initial radius of R and a translational velocity of V, the approximate value for the free rolling value of the rolling velocity is 𝜔 = 𝑉 (1+𝜀)𝑅, where 𝜀 is the hoop strain of the rolling tire. For a first guess, the hoop strain can be set to 0.0, and the rolling velocity will be within 10% of the actual value. After the first calculation, a smaller range bracketing the free rolling velocity should be used in a second calculation to refine the free rolling velocity. An accurate value of the free rolling velocity is necessary for subsequent analyses, such as varying the slip angle of the tire. A time varying slip angle can be specified by moving one of the nodes defining the direction vector of the translational velocity. To check that the stiffness scale factor in *CONTROL_STEADY_STATE_ROLLING is high enough, a complete cycle from a zero slip angle to a maximum value, then back to zero, should be performed. If the loading and unloading values are reasonably close, then the stiffness scale factor is adequate. Available options include: <BLANK> SET *LOAD_STIFFEN_PART Purpose: Staged construction. Available for solid, shell, and beam elements. Note: This keyword card is available starting in release 3 of version 971. Id Cards. Include as many of these cards as desired. This input ends at the next keyword (“*”) card. Card 1 1 2 3 4 5 6 7 8 Variable PID/PSID LC (blank) STGA STGR Type I Default none I 0 I 0 I 0 VARIABLE DESCRIPTION Part ID (or Part Set ID for the_SET option) Load curve defining factor vs. time Construction stage at which part is added (optional) Construction stage at which part is removed (optional) PID LC STGA STGR Remarks: 1. In many cases it is more convenient to use *DEFINE_STAGED_CONSTRUC- TION_PART which automatically generates *LOAD_STIFFEN_PART data. 2. For parts that are initially present but are excavated (removed) during the analysis, the stiffness factor starts at 1.0. During the excavation time, it ramps down to a small value such as 1.0E-6. The excavation time should be sufficient- ly long to avoid introducing shock or dynamic effects. For parts that are intro- duced during the construction, e.g. retaining walls, the elements are initially present in the model but the factor is set to a low value such as 1.0e-6. During the construction time the factor should be ramped up to 1.0. The construction time should be sufficiently long to avoid shock or dynamic effects. A factor that ramps up from 1.0E-6 to 1.0, then reduces back to 1.0E-6, can be used for tem- porary retaining walls, props, etc. 3. When the factor is increasing, it applies only to the stiffness and strength of the material in response to subsequent strain increments, not to any existing stress- es. 4. When the factor is decreasing, it applies also to existing stresses as well as to the stiffness and strength. 5. This feature works with all material models when used only to reduce the stiffness (e.g. parts that are excavated, not parts that are added during con- struction). It works for most material types in all other cases, except those few materials that re-calculate stresses each time step from total strains (elastic, SOIL_BRICK, rubber models, orthotropic elastic, fabric, etc). There is no error check at present to detect STIFFEN_PART being used with an inappropriate material model. Symptoms of resulting problems would include non-physical large stresses when a part stiffens, due to the accumulated strains in the “dormant” material since the start of the analysis. 6. This feature is generally used with *LOAD_GRAVITY_PART. The same curve is often used for the stiffness factor and the gravity factor. 7. There are 3 methods of defining the factor-versus-time: a) LC overrides all the other methods if non-zero b) STGA, STGR refer to stages at which the part is added and removed – the stages are defined in *DEFINE_CONSTRUCTION_STAGES. If STGA is zero, the part has full stiffness at time zero. If not, it ramps up from the small factor FACT (on *CONTROL_STAGED_CONSTRUCTION) up to 1.0 over the ramp time at the start of stage STGA. If STGR is zero, the stiffness factor continues at 1.0 until the end of the analysis. If not, it ramps down from 1.0 to FACT over the ramp time at the start of stage STGR. c) *DEFINE_STAGED_CONSTRUCTION_PART can be used instead of *LOAD_STIFFEN_PART to define this loading. During initialization, a *LOAD_STIFFEN_PART card will be created and the effect is the same as using the STGA, STGR method described above. *LOAD_SUPERPLASTIC_FORMING Purpose: Perform superplastic forming (SPF) analysis. This option can be applied to 2D and 3D solid elements and to 3D shell elements, and has been implemented for both explicit and implicit analyses. The pressure loading controlled by the load curve ID given below is scaled to maintain a constant maximal strain rate or other target value. This option must be used with material model 64, *MAT_RATE_SENSITIVE_POWER- LAW_PLASTICITY, for strain rate sensitive, powerlaw plasticity. For the output of data, see *DATA-BASE_SUPERPLASTIC_FORMING. Mass scaling is recommended in SPF applications. New options to compute the target value with various averaging techniques and autojump options to control the simulation are implemented. Strain-rate speedup is also available. See Remarks 5-7 for details. Card Sets. Include as many sets consisting of the following four cards as desired. This input ends at the next keyword (“*”) card. Card 1 1 2 3 4 5 6 7 8 Variable LCP1 CSP1 NCP1 LCP2 CSP2 NCP2 PCTS1 PCTS2 Type I I F I I F F F Default none none none. none none none 100.0 100.0 Remarks Card 2 1 2 3 1 4 1 5 1 6 7 Variable ERATE SCMIN SCMAX NCYL NTGT LEVEL TSRCH Type F F F Default none none none Remarks 27-98 (LOAD) I 0 2 I 1 I 0 5 F none 0.0 LS-DYNA R10.0 Card 3 1 2 3 4 5 6 7 8 Variable TPEAK TNEG TOSC POSC PDROP RILIM RDLIM STR Type F F F F F F F F Default 10.0 5.0 10.0 1.0 2.0 1.0 1.0 0.0 Remarks Card 4 1 2 3 4 5 6 7 Variable THRES LOWER UPPER TFACT NTFCT BOX Type F F F F I Default 5.0 90.0 99.0 1.0 10 I 0 Remarks 7 7 6 8 VARIABLE LCP1 CSP1 NCP1 LCP2 CSP2 DESCRIPTION Load curve number for Phase I pressure loading, . The scaled version of this curve as calculated by LS-DYNA is output to “curve1”. See Remark 3. Contact surface number to determine completion of Phase I. Percent of nodes in contact to terminate Phase I, . Load curve number for Phase II pressure loading (reverse), . The scaled version of this curve as calculated by LS-DYNA is output to “curve2”. See Remark 3. Contact surface to determine completion of Phase II, . NCP2 Percent of nodes in contact to terminate Phase II. *LOAD_SUPERPLASTIC_FORMING DESCRIPTION PCTS1 PCTS2 ERATE SCMIN SCMAX NCYL NTGT Percentage of nodes-in-contact to active autojump in Phase I forming. Percentage of nodes-in-contact to active autojump in Phase II forming. Desired target value. If it’s strain rate, this is the time derivative of the logarithmic strain. Minimum allowable value for load curve scale factor. To maintain a constant strain rate the pressure curve is scaled. In the case of a snap through buckling the pressure may be removed completely. By putting a value here the pressure will continue to act but at a value given by this scale factor multiplying the pressure curve. Maximum allowable value for load curve scale factor. Generally, it is a good idea to put a value here to keep the pressure from going to unreasonable values after full contact has been attained. When full contact is achieved the strain rates will approach zero and pressure will go to infinity unless it is limited or the calculation terminates. Number of cycles for monotonic pressure after reversal. Type of the target (controlling) variable: EQ.1: strain rate. EQ.2: effective stress. LEVEL Criterion to compute averaged maximum of controlling variable: EQ.0: no average used. GE.1: averaging over neighbors of element with peak value of controlling variable. This parameter determines the level of neighbor search. EQ.-1: averaging over elements within selective range of peak controlling variable. TSRCH Time interval to conduct neighbors search. AT Time when SPF Phase I simulation starts. TPEAK Additional run time to terminate simulation when maximum pressure is reached. VARIABLE DESCRIPTION TNEG TOSC POSC PDROP Additional run time to terminate simulation when percentage change of nodes-in-contact is zero or negative. Additional run time to terminate simulation when percentage change of nodes-in-contact oscillates within a specific value. Percentage change to define the oscillation of percentage of nodes-in-contact. Drop in percentage of nodes-in-contact from the maximum to terminate simulation after the specified termination percentage has been reached. STR Autojump option or strike-through time (period of time without autojump check): EQ.0: no autojump EQ.-1: autojump controlled by peak pressure EQ.-2: autojump controlled by percentage of nodes in contact EQ.-3: autojump controlled by both above GT.0: strike-through time, then same as STR = -3 THRES LOWER UPPER Threshold percentage that gives the threshold value above which elements are considered for average. Lower percentile of elements above the threshold value to be included for average. Upper percentile of elements above the threshold value to be included for average. RILIM Maximum percentage change for pressure increment. RDLIM Maximum percentage change for pressure decrement. TFACT Strain rate speedup factor. NTFCT Number of computing cycles to ramp up speedup. BOX Box ID or box set ID. See Remark 8. GT.0: box ID, see *DEFINE_BOX. LT.0: |BOX| is box set ID, see *SET_BOX. *LOAD_SUPERPLASTIC_FORMING 1. Optionally, a second phase can be defined. In this second phase a unique set of pressure segments must be defined whose pressure is controlled by load curve 2. During the first phase, the pressure segments of load curve 2 are inactive, and likewise, during the second phase the pressure segments of the first phase are inactive. When shell elements are used the complete set of pressure seg- ments can be repeated in the input with a sign reversal used on the load curve. When solid elements are used the pressure segments for each phase will, in general, must be unique. 2. This is an ad hoc parameter which should probably not be used. 3. There are three output files “pressure”, “curve1”, and “curve2” from the SPF simulation, and they may be plotted using ASCII > superpl in LS-PrePost. The file “curve2” is created only if the second phase is active. The time interval for writing out these files is controlled by *DATABASE_SUPERPLASTIC_FORM- ING. The files “curve1” and “curve2” contain the adjusted pressure histories calculated by SPF solver. File “pressure” contains time histories of scaling factor, maximal target value, averaged target value, and percentage of contact. 4. The constraint method contact, *CONTACT_CONSTRAINT_NODES_TO_SUR- FACE, is recommended for superplastic forming simulations since the penalty methods are not as reliable when mass scaling is applied. Generally, in super- plastic simulations mass scaling is used to enable the calculation to be carried out in real time. 5. In order to reduce the oscillation in pressure, the maximal target value used to adjust the pressure load is calculated by special averaging algorithm. There are two options available: a) Averaging over neighbors of element with maximum target value: In this meth- od, the element that has the maximum strain rate or other controlling var- iable is stored in each cycle of the computation. The elements close to the element with the maximum value are searched and stored in an array. The averaged maximal target value is computed over the neighboring el- ements. The user can input an integer number to control the level of neighbor search, which will affect the total number of elements for aver- age. Because the neighbor search is time consuming, the user can input a time interval to limit the occurrence of searching. The neighbor search is conducted only when the simulation time reaches the specified time or the element with maximum target value falls out of the array of neighbors. b) Averaging over elements within selective range of target value: In this method, all elements that have target value above a threshold value (a threshold percentage of maximum target value) are sorted according to their target value and the elements between the user specified lower percentile and upper percentile are selected to compute the average of the maximal tar- get value. 6. The SPF simulation can be controlled by various autojump options. When autojump conditions are met, the SPF simulation will be either terminated or continued from phase I to phase II simulation. The autojump check can be held inactive by setting a strikethrough time. In this case the SPF simulation will continue for that period of time and only be interrupted when the percentage of nodes-in-contact reaches 100% for a specified time. The available autojump conditions are: a) Peak pressure is reached and stays for certain time: The peak pressure is de- termined by the maximum allowable scale factor and the load curve. The simulation will continue for a user specified time before termination. b) User specified percentage of nodes-in-contact is reached: The simulation will be terminated or continued to Phase II automatically if one of the following conditions is met: i) ii) iii) iv) If the change of the percentage of nodes-in-contact is zero or nega- tive for a specified time. If the percentage of nodes-in-contact oscillates in a specified range for a specified time. If the percentage of nodes-in-contact drops more than a specified value from the maximum value recorded. If the percentage of nodes-in-contact reaches a user specified stop value. 7. 8. In order to speed up the simulation of the superplastic forming process, we scale down the computation time. By doing this we increase the strain rate allowed in the SPF process, resulting in reduced simulation time. However, caution should be utilized with this speedup as it may affect the accuracy of the results. We recommend no or small strain rate speedup for simulations with complex geometry or tight angles. If the user knows the area(s) in the workpiece that are critical in the SPF process, he can use the box option to limit the region(s) where the elements are checked for computing the average of the maximal target value. *LOAD_SURFACE_STRESS_{OPTION} Available options include: <BLANK> SET Purpose: This keyword modifies the behavior of shell elements causing them to pass pressure-type loads to material models 37 and 125 ; shells usually omit such effects. With this keyword, LS-DYNA calculates segment pressures from contact and applied pressure loads on both the upper and lower surfaces of the shell and applies them as negative local 𝑧-stresses during the simulation. It is found in some cases this capability can improve the accuracy of metal forming simulations. Card Sets. Include as many sets consisting of the following three cards as desired. This input ends at the next keyword (“*”) card. Card 1 1 2 3 4 5 6 7 8 Variable PID/PSID Type I Card 2 1 2 3 4 5 6 7 8 Variable LSCID1 LSCID2 LSCID3 LSCID4 LSCID5 LSCID6 LSCID7 LSCID8 Type I Card 3 1 I 2 I 3 I 4 I 5 I 6 I 7 I 8 Variable USCID1 USCID2 USCID3 USCID4 USCID5 USCID6 USCID7 USCID8 Type I I I I I I I VARIABLE DESCRIPTION PID/PSID Part ID or if option set is active, part set ID. Lower surface contact IDs. Up to eight IDs can be defined. These contacts definitions contribute to the pressure acting on the lower surface of the shell. If the pressure on the lower surface is due to applied pressure loads, specify a value -1 instead of a contact ID. Only one of the LSCIDn may be set to -1. Lower surface of a part is on the opposite side of the shell element normals, which must be made consistent (in LS-PrePost). Upper surface contact IDs. Up to eight IDs can be defined. These contacts definitions contribute to the pressure acting on the upper surface of the shell. . If the pressure on the upper surface is due to applied pressure loads, specify a value of -1 instead of a contact ID. Only one of the USCIDn may be set to -1. Upper surface of a part is on the same side of the shell element normals, which must be made consistent (in LS-PrePost). LSCIDn USCIDn Remarks: 1. MAT_TRANSVERSLY_ANISOTROPIC_ELASTIC_PLASTIC This keyword can be used with *MAT_037 when ETAN is set to a negative value , which triggers normal stresses (local 𝑧-stresses) resulting either from sliding contact or applied pressure to be considered in the shell formulation. The normal stresses can be significant in male die radius and corners in forming of Advanced High Strength Steels (AHSS). The negative local 𝑧-stresses are written to the d3plot files after Revision 97158, and can be plotted in LS-PrePost by selecting 𝑧-stress under FCOMP → Stress and select local under FCOMP. (37). 2. MAT_KINEMATIC_HARDENING_TRANSVERSLY_ANISOTROPIC (125). This keyword can also be used in a simulation with *MAT_125 to account for the normal stresses . For this material inserting this keyword anywhere in the input deck will invoke the shell normal stress calculation. *LOAD_THERMAL_OPTION Available options include: CONSTANT CONSTANT_ELEMENT_OPTION CONSTANT_NODE LOAD_CURVE TOPAZ VARIABLE VARIABLE_ELEMENT_OPTION VARIABLE_NODE VARIABLE_SHELL_OPTION Purpose: To define nodal temperatures that thermally load the structure. Nodal temperatures defined by the *LOAD_THERMAL_OPTION method are all applied in a structural only analysis. They are ignored in a thermal only or coupled ther- mal/structural analysis, see *CONTROL_THERMAL_OPTION. All the *LOAD_THERMAL options cannot be used in conjunction with each other. Only those of the same thermal load type, as defined below in column 2, may be used together. *LOAD_THERMAL_CONSTANT - Thermal load type 1 *LOAD_THERMAL_ELEMENT - Thermal load type 1 *LOAD_THERMAL_CONSTANT_NODE - Thermal load type 1 *LOAD_THERMAL_LOAD_CURVE - Thermal load type 2 *LOAD_THERMAL_TOPAZ - Thermal load type 3 *LOAD_THERMAL_VARIABLE - Thermal load type 4 *LOAD_THERMAL_VARIABLE_ELEMENT - Thermal load type 4 *LOAD_THERMAL_VARIABLE_NODE - Thermal load type 4 *LOAD_THERMAL_VARIABLE_SHELL - Thermal load type 4 *LOAD Purpose: Define nodal sets giving the temperature that remains constant for the duration of the calculation. The reference temperature state is assumed to be a null state with this option. A nodal temperature state, read in above and held constant throughout the analysis, dynamically loads the structure. Thus, the temperature defined can also be seen as a relative temperature to a surrounding or initial temperature. Card Sets. Include as many sets consisting of the following two cards as desired. This input ends at the next keyword (“*”) card. Card 1 1 2 3 4 5 6 7 8 Variable NSID NSIDEX BOXID Type I I Default none 0. I 0. 3 4 5 6 7 8 Card 2 Variable Type 1 T F Default 0. 2 TE F 0. VARIABLE DESCRIPTION NSID Nodal set ID containing nodes for initial temperature EQ.0: all nodes are included: NSIDEX BOXID Nodal set ID containing nodes that are exempted from the imposed temperature (optional). All nodes in box which belong to NSID are initialized. Others are excluded (optional). T Temperature *LOAD_THERMAL_CONSTANT DESCRIPTION TE Temperature of exempted nodes (optional) *LOAD_THERMAL_CONSTANT_ELEMENT_OPTION Available options include: BEAM SHELL SOLID TSHELL Purpose: Define a uniform element temperature that remains constant for the duration of the calculation. The reference temperature state is assumed to be a null state. An element temperature, read in above and held constant throughout the analysis, dynamically loads the structure. The defined temperature can also be seen as a relative temperature to a surrounding or initial temperature. Element Cards. Include as many cards in this format as desired. This input ends at the next keyword (“*”) card. 3 4 5 6 7 8 Card 1 1 Variable EID Type I 2 T F Default none 0. VARIABLE DESCRIPTION Element ID Temperature, see remark below. EID T Remarks: 1. The temperature range for the constitutive constants in the thermal materials must include the reference temperature of zero. If not termination will occur with a temperature out-of-range error immediately after the execution phase is entered. *LOAD_THERMAL_CONSTANT_NODE Purpose: Define nodal temperature that remains constant for the duration of the calculation. The reference temperature state is assumed to be a null state with this option. A nodal temperature state, read in above and held constant throughout the analysis, dynamically loads the structure. Thus, the temperature defined can also be seen as a relative temperature to a surrounding or initial temperature. Node Cards. Include as many cards in this format as desired. This input ends at the next keyword (“*”) card. 3 4 5 6 7 8 Card 1 Variable NID Type I 2 T F Default none 0. VARIABLE DESCRIPTION Node ID Temperature, see remark below. NID T Remarks: 1. The temperature range for the constitutive constants in the thermal materials must include the reference temperature of zero. If not termination will occur with a temperature out-of-range error immediately after the execution phase is entered. *LOAD Purpose: Temperatures computed in a prior thermal-only analysis are used to load a mechanical-only analysis. The rootname of the d3plot database from the thermal-only analysis is specified on the execution line of the mechanical-only analysis using T = tpf, where tpf is that rootname, e.g., T = d3plot. Warnings: 1.If using a double precision LS-DYNA executable in making the two runs, do not write the d3plot data using 32ieee format in the thermal-only run, i.e., the envi- ronment variable LSTC_BINARY must not be set. 2.The rootnames of the d3plot databases from the two runs must not conflict. Such conflict can be avoided, for example, by using jobid = jobname on the execution line of the second (mechanical-only) run. *LOAD_THERMAL_LOAD_CURVE Purpose: Nodal temperatures will be uniform throughout the model and will vary according to a load curve. The temperature at time = 0 becomes the reference temperature for the thermal material. The reference temperature is obtained from the optional curve for dynamic relaxation if this curve is used. The load curve option for dynamic relaxation is useful for initializing preloads. Thermal Load Curve Cards. Include as many cards in this format as desired. This input ends at the next keyword (“*”) card. Card 1 2 3 4 5 6 7 8 Variable LCID LCIDDR Type I Default none I 0 VARIABLE LCID DESCRIPTION Load curve ID, see *DEFINE_CURVE, to define temperature versus time. LCIDDR An optional load curve ID, see *DEFINE_CURVE, to define temperature versus time during the dynamic relaxation phase. *LOAD Purpose: Nodal temperatures will be read in from the TOPAZ3D database. This file is defined on the execution line by the specification: T = tpf, where tpf is a binary database file (e.g., T3PLOT). *LOAD_THERMAL_VARIABLE Purpose: Define nodal temperature using node set(s) and temperature vs. time curve(s). Card Sets. Include as many sets consisting of the following two cards as desired. This input ends at the next keyword (“*”) card. Card 1 1 2 3 4 5 6 7 8 Variable NSID NSIDEX BOXID Type I I Default none 0. I 0. Card 2 Variable 1 TS Type F 2 TB F 3 4 5 6 7 8 LCID TSE TBE LCIDE LCIDR LCIDEDR I F F I I I Default 0. 0. none 0. 0. none none none Remark 1 1 1 1 1 VARIABLE DESCRIPTION NSID Nodal set ID containing nodes : EQ.0: all nodes are included. NSIDEX BOXID Nodal set ID containing nodes that are exempted (optional), . All nodes in box which belong to NSID are initialized. Others are excluded. TS TB Scaled temperature. Base temperature. VARIABLE DESCRIPTION LCID TSE TBE LCIDE LCIDR Load curve ID that multiplies the scaled temperature, . Scaled temperature of the exempted nodes (optional). Base temperature of the exempted nodes (optional). Load curve ID that multiplies the scaled temperature of the exempted nodes (optional), . Load curve ID that multiplies the scaled temperature during the dynamic relaxation phase LCIDEDR Load curve ID that multiplies the scaled temperature of the exempted nodes (optional) during the dynamic relaxation phase. Remarks: 1. The total temperature is defined as 𝑇 = TB + TS × 𝑓 (𝑡) where 𝑓 (𝑡) is the current value of the load curve, TS is the scaled temperature, and TB is the base temperature. The rate of thermal strain is based on the rate of temperature change. In other words, the thermal load arises from change in total temperature. Furthermore, the calculation of the thermal strain from the coefficient of thermal expansion depends on the material model, and some material models, e.g., *MAT_255, may offer multiple options. Temperature-dependent material properties are based on the total temperature. *LOAD_THERMAL_VARIABLE_BEAM_{OPTION} Available options include: <BLANK> SET Purpose: Define a known temperature time history as a function of the section coordinates for beam elements. To set the temperature for the whole element see *LOAD_THERMAL_VARIABLE_ELEMENT_BEAM. Card 1 Variable 1 ID 2 3 4 5 6 7 8 EID/SID IPOLAR Type I I Default none none 1 0 Temperature Cards. Include as many cards in the following format as desired. This input ends at the next keyword (“*”) card. Card 2 1 2 3 4 5 6 7 8 Variable TBASE TSCALE TCURVE TCURDR SCOOR TCOOR Type Default F 0 F I I F F 1.0 0 TCURVE none none VARIABLE DESCRIPTION ID Load case ID EID/SID Beam ID or beam set ID IPOLAR GT.0: the coordinates SCOOR and TCOOR are given in polar coordinates TBASE Base temperature t t 10 11 12 S = -1, T=+1 S=+1, T=+1 s s S = -1, T = -1 S=+1, T = -1 Figure 0-1. Figure illustrating point ordering. VARIABLE DESCRIPTION TSCALE Constant scale factor applied to temperature from curve TCURVE Curve ID for temperature vs. time TCURDR Curve ID for temperature vs. time used during dynamic relaxation SCOOR Normalized coordinate in local s-direction (-1.0 to +1.0) TCOOR Normalized coordinate in local t-direction (-1.0 to +1.0) Remarks: 1. The temperature T is defined as: T = TBASE + TSCALE × 𝑓 (𝑡) where 𝑓 (𝑡) is the current ordinate value of the curve. If the curve is undefined, then T = TBASE at all times. 2. At least four points (four Card 2’s) must be defined in a rectangular grid. The required order of the points is as shown in Figure 0-1. First, define the bottom row of points (most negative t), left to right in order of increasing s. Then in- crement t to define the next row of points, left-to-right in order of increasing s, and so on. The s-t axes are in the plane of the beam cross-section with the s-axis in the plane of nodes N1, N2, N3 defined in *ELEMENT_BEAM. 3. For the polar option, SCOOR is the non-dimensional radius 𝑅/𝑅0 where 𝑅0 is the outer radius of the section; and TCOOR is defined as θ/π, where θ is the angle in radians from the s-axis, defined in the range –π < θ < π. 4. Temperatures will be assigned to the integration points by linear interpolation from the points defined using this command. *LOAD_THERMAL_VARIABLE_ELEMENT_OPTION Available options include: BEAM SHELL SOLID TSHELL Purpose: Define element temperature that is variable during the calculation. The reference temperature state is assumed to be the temperature at time = 0.0 with this option. Element Cards. Include as many cards in the following format as desired. This input ends at the next keyword (“*”) card. Card 1 Variable EID Type I 2 TS F 3 TB F 4 5 6 7 8 LCID I Default none 0. 0. none VARIABLE DESCRIPTION Element ID Scaled temperature Base temperature Load curve ID defining a scale factor that multiplies the scaled temperature as a function of time, . EID TS TB LCID Remarks: 1. The temperature is defined as: 𝑇 = TB + TS × 𝑓 (𝑡) where 𝑓 (𝑡) is the current value of the load curve, TS is the scaled temperature, and TB is the base temperature *LOAD_THERMAL_VARIABLE_NODE Purpose: Define nodal temperature that is variable during the calculation. The reference temperature state is assumed to be a null state with this option. A nodal temperature state read in and varied according to the load curve dynamically loads the structure. Thus, the defined temperatures are relative temperatures to an initial reference temperature. Node Cards. Include as many cards in the following format as desired. This input ends at the next keyword (“*”) card. Card 1 Variable NID Type I 2 TS F 3 TB F 4 5 6 7 8 LCID I Default none 0. 0. none VARIABLE DESCRIPTION NID Node ID Scaled temperature Base temperature Load curve ID that multiplies the scaled temperature, . TS TB LCID Remarks: 1. The temperature is defined as: 𝑇 = TB + TS × 𝑓 (𝑡) where 𝑓 (𝑡) is the current value of the load curve, TS is the scaled temperature, and TB is the base temperature *LOAD_THERMAL_VARIABLE_SHELL_{OPTION} Available options include: <BLANK> SET Purpose: Define a known temperature time history as a function of the through- thickness coordinate for the shell elements. Card 1 Variable 1 ID 2 3 4 5 6 7 8 EID/SID Type I I Default none none Temperature Cards. Include as many cards of this type as desired. This input ends at the next keyword (“*”) card. Card 2 1 2 3 4 5 6 7 8 Variable TBASE TSCALE TCURVE TCURDR ZCO Type Default F 0 F 1.0 I 0 I F TCURVE -1/+1 VARIABLE DESCRIPTION ID Load case ID EID/SID Shell ID or shell set ID TBASE Base temperature TSCALE Constant scale factor applied to temperature from curve TCURVE Curve ID for temperature vs. time VARIABLE TCURDR DESCRIPTION Curve ID for temperature vs. time used during dynamic relaxation ZCO Normalized through-thickness coordinate (-1.0 to +1.0) Remarks: 1. The temperature T is defined as: 𝑇 = TBASE + TSCALE × 𝑓 (𝑡) where 𝑓 (𝑡) is the current ordinate value of the curve. If the curve is undefined, then T = TBASE at all times. 2. Through-thickness points must be defined in order of increasing ZCO (-1.0 to +1.0). ZCO=+1.0 is the top surface of the element, i.e. the element surface in the positive outward normal vector direction from the mid-plane. 3. At least two points (two Card 2’s) must be defined. Temperatures will be assigned in the through-thickness direction by linear interpolation from the points defined using this command. 4. 5. If the element has multiple in-plane integration points, the same temperature distribution is used at each in-plane integration point. If a shell’s temperature distribution is defined using this card, any values defined by *LOAD_THERMAL_NODE are ignored for that shell. *LOAD_VOLUME_LOSS Purpose: To represent the effect of tunneling on surrounding structures, it is common to assume that a pre-defined fraction (e.g., 2%) of the volume occupied by the tunnel is lost during the construction process. This feature is available for solid elements only. Part Set Cards. Include as many of these cards as desired. This input ends at the next keyword (“*”) card. Card 1 2 3 Variable PSID COORD LCUR Type I Default none I 0 I 0 4 FX F 1 5 FY F 1 6 FZ F 1 7 8 PMIN FACTOR F F -1.e20 .01 VARIABLE DESCRIPTION PSID Part Set ID COORD Coordinate System ID (default - global coordinate system) LCUR Curve ID containing volume fraction lost vs. time FX FY FZ Fraction of strain occurring in x-direction Fraction of strain occurring in 𝑦-direction Fraction of strain occurring in 𝑧-direction PMIN (Leave blank) FACTOR Feedback factor Remarks: Volume loss is modeled by a process similar to thermal contraction: if the material is unrestrained it will shrink while remaining unstressed; if restrained, stresses will become more tensile. Typically the material surrounding the tunnel offers partial restraint; the volume loss algorithm adjusts the applied “thermal” strains to attempt to achieve the desired volume loss. Optionally, FX, FY and FZ may be defined: these will be treated as ratios for the 𝑥, 𝑦 and 𝑧 strains; this feature can be used to prevent contraction parallel to the tunnel axis. The total volume of all the parts in the part set is monitored and output at the time- history interval (on *DATABASE_BINARY_D3THDT) to a file named vloss_output. This file contains lines of data (time, volume1, volume2, volume3…) where volume1 is the total volume of elements controlled by the first *LOAD_VOLUME_LOSS card, volume2 is the total volume of elements controlled by the second *LOAD_VOLUME_LOSS card, etc. This feature works only with material types that use incremental strains to compute stresses. Thus, hyperelastic materials (e.g. MAT_027) are excluded, as are certain foam material types (e.g. MAT_083). The feedback factor controls how strongly the algorithm tries to impose the desired change of volumetric strain. The default value is recommended. If the volumetric response appears noisy or unstable, it may be necessary to reduce FACTOR. Alternatively, if the actual volumetric strain changes much more slowly than the input curve, it may be necessary to increase FACTOR. The keyword *MODULE provides a way to load user compiled libraries at runtime, to support user defined capabilities such as material models, equations of state, element formulations, etc. The following keywords implement this capability: *MODULE_LOAD *MODULE_PATH *MODULE_USE *MODULE Purpose: Load a dynamic library for user subroutines. Card Sets. Repeat as many sets data cards as desired (cards 1 and 2) to load multiple libraries. This input ends at the next keyword (“*”) card. Card 1 1 2 3 4 5 6 7 8 Variable MDLID Type A20 Default none TITLE A60 none Card 2 1 2 3 4 5 6 7 8 Variable Type Default FILENAME C none VARIABLE DESCRIPTION MDLID Module identification. A unique string label must be specified. TITLE Description of the module. FILENAME File name of the library to be loaded, 80 characters maximum. If the filename has no path component, LS-DYNA will search in all directories specified in *MODULE_PATH first. If not found and the filename starts with “+” (a plus sign), LS-DYNA will continue to search all directories specified in the system environment variable LD_LIBRARY_PATH. *MODULE_LOAD 1. The MODULE capability described here and in *MODULE_USE is still under development and is considered experimental. As such, it is currently only supported in specially compiled executables on Linux systems 2. is option library If only one dynamic loaded and no rules are required (*MODULE_USE), this dynamic library can be specified through the execution line variable The LD_LIBRARY_PATH is also used for searching the dynamic library if the file- name starts with “+”. This execution line option provides the support to the classic user subroutine subroutines without modifying the input deck. “module = dll”. environment system *MODULE_PATH_{OPTION} *MODULE_PATH_{OPTION} Available options: <BLANK> RELATIVE *MODULE LS-DYNA’s default behavior is search for modules in the current working directory. If a module file is not found and the filename has no path component, LS-DYNA will search in all directories specified on the cards following a *MODULE_PATH keyword. Multiple paths can specified using one *MODULE_PATH keyword card, i.e., *MODULE_PATH Directory_path1 Directory_path2 Directory_path3 Directory paths are read until the next “*” card is encountered. A directory path can have up to 236 characters. See Remark 3. When the RELATIVE option is used, all directories are relative to the location of the input file. For example, if “i=/home/test/problems/input.k” is given on the command line, and the input contains *MODULE_PATH_RELATIVE lib ../lib then the two directories /home/test/problems/lib and /home/test/lib will be searched for module files. Remarks: 1. Filenames and pathnames are limited to 236 characters spread over up to three 80 character lines. When 2 or 3 lines are needed to specify the filename or pathname, end the preceding line with "˽+" (space followed by a plus sign) to signal that a continuation line follows. Note that the "˽+" combination is, itself, part of the 80 character line; hence the maximum number of allowed characters is 78 + 78 + 80 = 236. *MODULE_USE Purpose: Define the rules for mapping the user subroutines loaded in dynamic libraries to the model. The rules can be applied to: *MAT_USER_DEFINED_MATERIAL_MODELS (MAT 41 - 50) *MAT_THERMAL_USER_DEFINED *EOS_USER_DEFINED *SECTION_SOLID *SECTION_SHELL (MAT T11 - T15) (EOS 21 – 30) (ELFORM 101 - 105) (ELFORM 101- 105) and other subroutines in the LS-DYNA user subroutine package. LS-DYNA requires that subroutines in modules be named as if they were part of the traditional user subroutine framework. Each module, however, can contain a complete set of those subroutines, and it is, therefore, possible to import in different modules the same subroutines of the same name several times. Each module is, essentially, an independent copy of the traditional user-subroutine framework. This keyword, *MODULE_USE, deals with namespace conflicts by defining how each subroutine in the module is presented to the other keywords. The rules defined in *MODULE_USE are applied to only one dynamic library. Card 1 1 2 3 4 5 6 7 8 Variable MDLID Type A20 Default none Rule Cards. Card 2 defines rules for the module specified in Card 1. Include one instance of this card for each subroutine to be mapped. If two rules conflict, new rules override existing rules. Input ends at the next keyword (“*”) card. Card 2 1 2 3 4 5 6 7 8 Variable TYPE PARAM1 PARAM2 Type A20 A20 A20 Default none blank blank VARIABLE DESCRIPTION MDLID Module identification defined in *MODULE_LOAD. TYPE Rule type. See TYPE definitions below. PARAM1 Type dependent parameter. PARAM2 Type dependent parameter. User Defined Materials: TYPE UMAT DESCRIPTION Implements the user material type PARAM1 in the model via a possibly different type PARAM2 in the dynamic library. Types in the extended range from 1001 to 2000 can be used as material types in the model. For example, if PARAM1 = 1001 and PARAM2 = 42, then model material 1001 will use subroutine umat42 from this library. If PARAM1 is blank and PARAM2 is not, then all user materials in the model will use the indicated subroutine from this library. If PARAM2 is blank and PARAM1 is not, the material type PARAM1 in the model will use the traditional subroutine from this library. For example, if PARAM1 = 43 and PARAM2 is blank, then material type 43 in the model will use the subroutine umat43 from this library If both PARAM1 and PARAM2 are blank, then all user defined MATID *MODULE_USE DESCRIPTION materials in the model will use the traditional subroutines from this library (41 → umat41, 42 → umat42, etc). Implements the user material having ID = PARAM1 via a possibly different material type PARAM2 in the dynamic library. PARAM2 may be blank if the material type defined in the model is the same as the one in the dynamic library. PARAM1 can be a numerical id or label of the material as defined in the model. Materials beyond user material models can be overloaded. Thermal User Defined Materials: TYPE TUMAT TMATID DESCRIPTION Implements the user thermal material type PARAM1 in the model (PARAM1 = 11-15) via type PARAM2 in the dynamic library. See type UMAT for the default rules. Implements the user thermal material having ID = PARAM1 via thermal material type PARAM2 in the dynamic library. PARAM2 may be blank if the material type defined in the model is the same as the one in the dynamic library. PARAM1 can be a numerical id or label of the thermal material as defined in the model. Materials beyond user material models can be overloaded. User Defined EOS: TYPE UEOS DESCRIPTION Implements the user EOS model PARAM1 in the model (PARAM1 = 21-30) via EOS model PARAM2 in the dynamic library. See type UMAT for the default rules. User Defined Elements: TYPE UELEM DESCRIPTION Implements the user element type PARAM1 in the model (PARAM1 = 101-105) via element type PARAM2 in the dynamic library. See type UMAT for the default rules. SECTIONID *MODULE DESCRIPTION Implements the user element type with section ID = PARAM1 via element type PARAM2 in the dynamic library. PARAM2 may be blank if the element type defined in the model is the same as the one in the dynamic library. Note: Solid element types are mapped to subroutine usrsld, and shell element types are mapped to sub- routine usrshl. These interfaces are documented in dyn21b.f. Other User Subroutines: TYPE DESCRIPTION The following subroutines implemented in the dynamic library are used for the model. Any subroutines with the same name in other dynamic libraries, if they exist, are ignored. UMATFAIL matusr_24 matusr_103 UFRICTION usrfrc UWEAR UADAP UWELDFAIL USPH UTHERMAL ULOAD userwear useradap uadpnorm uadpval uweldfail uweldfail12 uweldfail22 hdot usrhcon usrflux ujntfdrv loadsetud loadud UELEMFAILCTL LS-DYNA R10.0 matfailusercontrol *MODULE_USE DESCRIPTION UMATFPERT usermatfpert UREBAR rebar_bondslip_get_nhisvar rebar_bondslip_get_force ULAGPOROUS lagpor_getab_userdef UAIRBAG UALE UCOUPLE2OTHER airusr user_inflator al2rfn_criteria5 al2rmv_criteria5 alerfn_criteria5 alermv_criteria5 shlrfn_criteria5 shlrmv_criteria5 sldrfn_criteria5 sldrmv_criteria5 f3dm9ale_userdef1 couple2other_boxminmax couple2other_comm couple2other_dt couple2other_extra couple2other_getf couple2other_givex couple2other_reader chkusercomm usercomm usercomm1 UOUTPUT ushout Remarks: 1. In order to simplify the development of user defined materials via modules, the *MODULE_USE keyword can be omitted in one special case. If only a single module library will be used and no remapping of material types is desired, then a *MODULE_LOAD keyword may appear with a single library and no other *MODULE keywords. In this case, all the user defined subroutines found in this library will be used in the normal way. For example, if the library contains umat41 and umat43, those routines will be used for all materials of type 41 and 43 respectively, and the *MODULE_USE keyword describing this may be omit- ted. *MODULE The following examples demonstrate the input for the MODULE keywords: *MODULE_PATH *MODULE_LOAD *MODULE_USE $$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ $ $ Using *MODULE_PATH to define additional directories where $ dynamic libraries are saved. $ $------------------------------------------------------------------------------ $ *MODULE_PATH /home/lsdynauser/lib $ $$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ $ $ Using *MODULE_LOAD to load all dynamic libraries for this model. $ $ three libraries are loaded here for demonstration: $ $ M_LIB: my own library which is under development. A debug version is built $ in my local directory. $ it contains: UMAT41, UMAT42, and UMAT45 $ $ LIB_A: a hypoelastic model, provided by a third party, for shell & solid. $ it contains UMAT41 only, with an optional FLUID $ $ LIB_B: contains two material models provided by another company, with $ UMAT41: a elasto-plastic model $ UMAT45: a hyper-elastic model for rubber $ $------------------------------------------------------------------------------ *MODULE_LOAD $...>....1....>....2....>....3....>....4....>....5....>....6....>....7....>....8 M_LIB My own library /my_development_path/mylib_r123_dbg.so LIB_A library from company A Lib_hypoelastic.so LIB_B library from company B Lib_plastic.so $ $$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ $ $ Using *MODULE_USE to map to user subroutines $ $ CASE 1: $ $ M_LIB is used for UMAT41,UMAT42,UMAT45 in the model, as default $ UMAT41 in LIB_A is used for MT=1001 in the model for shell, and MT=1002 for solid $ UMAT45 in LIB_B is used for MATID=202, which also happens to hvae MT=1002 $ *MODULE_USE M_LIB $...>....1....>....2....>....3....>....4....>....5....>....6....>....7....>....8 UMAT *MODULE_USE LIB_A $...>....1....>....2....>....3....>....4....>....5....>....6....>....7....>....8 UMAT 1001 41 UMAT 1002 41 *MODULE_USE LIB_B $...>....1....>....2....>....3....>....4....>....5....>....6....>....7....>....8 MATID 202 45 $$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ $ CASE 2: $ $ M_LIB is used for UMAT41,UMAT42 as, $ MATID=101 with MT=41 $ MATID=102 with MT=42 $ UMAT45 in LIB_B is used with different material properties, as, $ MATID=201 with MT=1001 $ MATID=202 with MT=1002 $ MATID=203 with MT=1003 $ *MODULE_USE LIB_B $...>....1....>....2....>....3....>....4....>....5....>....6....>....7....>....8 UMAT 45 *MODULE_USE M_LIB $...>....1....>....2....>....3....>....4....>....5....>....6....>....7....>....8 MATID 101 MATID 102 *NODE *NODE_{OPTION} *NODE_MERGE_SET *NODE_MERGE_TOLERANCE *NODE_RIGID_SURFACE *NODE_SCALAR_{OPTION} *NODE_THICKNESS *NODE_TO_TARGET_VECTOR *NODE_TRANSFORM Available options include: <BLANK> MERGE *NODE Purpose: Define a node and its coordinates in the global coordinate system. Also, the boundary conditions in global directions can be specified. Generally, nodes are assigned to elements; however, exceptions are possible, see remark 2 below. The nodal point ID must be unique relative to other nodes defined in the *NODE section. The MERGE option is usually applied to boundary nodes on disjoint parts and only applies to nodes defined when the merge option is invoked. With this option, nodes with identical coordinates are replaced during the input phase by the first node encountered that shares the coordinate. During the merging process a tolerance is used to determine whether a node should be merged. This tolerance can be defined using the keyword *NODE_MERGE_TOLERANCE keyword, which is recommended over the default value. See the *NODE_MERGE_TOLERANCE input description in the next section. Node Cards. Include as many cards in the following format as desired. This input ends at the next keyword (“*”) card. Card 1 1 2 3 4 5 6 7 Variable NID Type I X F Default none 0. Remarks Y F 0. Z F 0. 10 8 TC 9 RC F F 0. 0. 1 1 VARIABLE DESCRIPTION NID Node number X Y Z x coordinate y coordinate z coordinate VARIABLE DESCRIPTION TC Translational Constraint: EQ.0: no constraints, EQ.1: constrained x displacement, EQ.2: constrained y displacement, EQ.3: constrained z displacement, EQ.4: constrained x and y displacements, EQ.5: constrained y and z displacements, EQ.6: constrained z and x displacements, EQ.7: constrained x, y, and z displacements. RC Rotational constraint: EQ.0: no constraints, EQ.1: constrained x rotation, EQ.2: constrained y rotation, EQ.3: constrained z rotation, EQ.4: constrained x and y rotations, EQ.5: constrained y and z rotations, EQ.6: constrained z and x rotations, EQ.7: constrained x, y, and z rotations. Remarks: 1. Boundary conditions can also be defined on nodal points in a local (or global) system by using the keyword *BOUNDARY_SPC. For other possibilities also see the *CONSTRAINED keyword section of the manual. 2. A node without an element or a mass attached to it will be assigned a very small amount of mass and rotary inertia. Generally, massless nodes should not cause any problems but in rare cases may create stability problems if these massless nodes interact with the structure. Warning messages are printed when massless nodes are found. Also, massless nodes are used with rigid bod- ies to place joints, see *CONSTRAINED_EXTRA_NODES_OPTION and *CON- STRAINED_NODAL_RIGID_BODY. *NODE_MERGE_SET Purpose: The MERGE_SET option is applied to a set of boundary nodes on disjoint part. With this option, nodes with identical coordinates that are members of any node set ID defined by this keyword are replaced during the input phase by one node within the set or sets. Of the nodes sharing the same coordinates, the node chosen is the one with the smallest ID. During the merging process a tolerance is used to determine whether a node should be merged. This tolerance can be defined using the keyword *NODE_MERGE_TOLERANCE keyword, which is recommended over the default value. See the *NODE_MERGE_TOLERANCE input description in the next section. Only nodes contained within the specified sets will be merged. Nodes contained within the set are defined by the *NODE keyword. With this option, the keyword *NODE_- MERGE is not needed. Node Set Cards. Include as many cards as desired. This input ends at the next keyword (“*”) card. Card 1 1 2 3 4 5 6 7 8 Variable NSID Type I Default none VARIABLE DESCRIPTION NSID Node set ID containing list of nodes to be considered for merging. *NODE Purpose: Define a tolerance is determine whether a node should be merged for the keyword, *NODE_MERGE. Card 1 1 2 3 4 5 6 7 8 Variable TOLR Type F Default yes VARIABLE TOLR Remarks: DESCRIPTION Physical distance used to determine whether to merge a nodal pair of nearby nodes. See remark below. If the tolerance, TOLR, is undefined or if it is defaulted to zero, a value is computed as: TOLR = 10−5 ⋅ XMAX + YMAX + ZMAX − XMIN − YMIN − ZMIN 3 × √NUMNP where XMIN, XMAX, YMIN,YMAX, ZMIN, and ZMAX represent the minimum and maximum values of the (x,y,z) nodal point coordinates in the global coordinate system, and NUMNP is the number of nodal points. *NODE_RIGID_SURFACE Purpose: Define a rigid node and its coordinates in the global coordinate system. These nodes are used to define rigid road surfaces and they have no degrees of freedom. The nodal points are used in the definition of the segments that define the rigid surface. See *CONTACT_RIGID_SURFACE. The nodal point ID must be unique relative to other nodes defined in the *NODE section. Node Cards. Include as many cards in the following format as desired. This input ends at the next keyword (“*”) card. Card 1 1 2 3 4 5 6 7 8 9 10 Variable NID Type I X F Default none 0. Remarks Y F 0. Z F 0. VARIABLE DESCRIPTION NID Node number X Y Z x coordinate y coordinate z coordinate Available options include: <BLANK> VALUE *NODE Purpose: Define a scalar nodal point which has one degree-of-freedom. The scalar point ID must be unique relative to other nodes defined in the *NODE section. Node Card. Card 1 for no keyword option (option set to <BLANK>). Include as many cards in the following format as desired. This input ends at the next keyword (“*”) card. Card 1 1 2 3 4 5 6 7 8 9 10 Variable NID NDOF Type I I Default none 0 Node Card. Card 1 for the VALUE keyword option. Include as many cards in the following format as desired. This input ends at the next keyword (“*”) card. Card 1 1 Variable NID Type I Default none 2 X1 F 0 3 X2 F 0 4 X3 F 0 5 6 7 NDOF I 0 VARIABLE DESCRIPTION NID Scalar node ID. *NODE_SCALAR DESCRIPTION NDOF Number of degrees-of-freedom EQ.0: fully constrained EQ.1: one degree-of-freedom EQ.2: two degrees-of-freedom EQ.3: three degrees-of-freedom XI Initial value of Ith degree of freedom. *NODE_THICKNESS_{OPTION1}_{OPTION2} For OPTION1 the available options include: <BLANK> SET For OPTION2 the available options include: <BLANK> GENERATE Purpose: Define nodal thickness that overrides nodal thickness otherwise determined via *SECTION_SHELL, *PART_COMPOSITE, or *ELEMENT_SHELL_THICKNESS. The option GENERATE generates a linear thickness distribution between a starting node (or node set) and a ending node (or node set). Card 1 1 2 3 4 5 6 7 8 Variable ID1 THK ID2 INC Type I F I I Default none none none none VARIABLE DESCRIPTION Node ID, or node set ID if SET option is active. If GENERATE option is active, ID1 serves as the starting node (or node set). Thickness at node ID1, or node set ID1 if SET option is active (ignored if GENERATE option is active). Ending node (or node set) if GENERATE option is active. Increment in node numbers if GENERATE option is active. ID1 THK ID2 INC Remarks: When the GENERATE option is active, both the starting and ending nodes (or node sets) must have a nodal thickness as defined by *NODE_THICKNESS or NODE_- THICKNESS_SET. The sample commands shown below create a linear thickness distribution between node set 100 and node set 200. *SET_NODE_LIST 100 1, 15, 39 *SET_NODE_LIST 200 7, 21, 45 *NODE_THICKNESS_SET $ assign thickness of 2.0 to node 1, 15 and 39 100, 2.0 *NODE_THICKNESS_SET $ assign thickness of 5.0 to node 7, 21 and 45 200, 5.0 *NODE_THICKNESS_SET_GENERATE $ assign thickness of 3. (= 2.+1.) to node 3 (=1+2), 17 (=15+2) and 41 (=39+2) $ assign thickness of 4. (= 2.+2.) to node 5 (=1+4), 19 (=15+4) and 43 (=39+4) 100,, 200, 2 *NODE Purpose: Calculate vector components of the normal distance from the target to a node from target. fitted of a part best *CONTROL_FORMING_BESTFIT_VECTOR. This keyword is generated the to Node Cards. Include as many cards in the following format as desired. This input ends at the next keyword (“*”) card. Card 1 1 2 3 4 5 6 7 8 9 10 Variable NID XDELTA YDELTA ZDELTA Type I Default none F 0. F 0. F 0. VARIABLE DESCRIPTION NID Node ID on a part best fitted to the target. Difference in X-coordinates of the normal distance from the target (typically scan data) to a node of a part best fitted to the target. Difference in Y-coordinates of the normal distance from the target (typically scan data) to a node of a part best fitted to the target. Difference in Z-coordinates of the normal distance from the target (typically scan data) to a node of a part best fitted to the target. XDELTA YDELTA ZDELTA Remarks: 1. This keyword from *CONTROL_FORMING_BESTFIT_VECTOR and is available starting from Revision 112655. automatically generated is *NODE_TRANSFORM Purpose: Perform a transformation on a node set based on a transformation defined by the keyword *DEFINE_TRANSFORMATION. Transformation Cards. Include as many cards in the following format as desired. This input ends at the next keyword (“*”) card. Card 1 1 2 3 4 5 6 7 8 Variable TRSID NSID Type I I Default none none VARIABLE TRSID DESCRIPTION The ID of the transformation defined under *DEFINE_TRANS- FOR-MATION. NSID Node set ID of the set of nodes to be subject to the transformation. The *PARAMETER family of commands assign numerical values or expressions to named parameters. The parameter names can be used subsequently in the input in place of numerical values. *PARAMETER_OPTION *PARAMETER_DUPLICATION *PARAMETER_EXPRESSION *PARAMETER_TYPE *PARAMETER_{OPTION}_{OPTION} The available options are <BLANK> LOCAL MUTABLE Purpose: Define the numerical values of parameter names referenced throughout the input file. The parameter definitions, if used, should be placed at the beginning of the input file following *KEYWORD or at the beginning of an include file if the LOCAL option is specified. Parameter Cards. Include as many cards as necessary. Card 1 1 2 3 4 5 6 7 8 Variable PRMR1 VAL1 PRMR2 VAL2 PRMR3 VAL3 PRMR4 VAL4 Type A I, F or C A I, F or C A I, F or C A I, F or C Default none none none none none none none none VARIABLE DESCRIPTION PRMRn PRMRn sets both the nth parameter and its storage type. PRMR = T xxxxxxxxx ⏟⏟⏟⏟⏟⏟⏟ 9 character name The first character, “T”, is decoded as follows: T.EQ.“R”: Parameter is a real number T.EQ.“I”: Parameter is an integer T.EQ.“C”: Parameter is a character The remaining 9 characters specifiy the name of the parameter. A parameter name “time” (case insensitive) is disallowed. For example, to define a shell thickness named, "SHLTHK", the input “RSHLTHK”, “R␣␣␣SHLTHK”, or “R␣␣SHLTHK␣” are all equivalent 10 character strings (“␣” is space). For instructions regard how to use the variable “SHLTHK” see Remark 1. Define the value of the nth parameter as either a real or integer number, or a character string consistent with preceding definition for PRMRn. *PARAMETER VARIABLE VALn Remarks: 1. Syntax for Using Parameters. Parameters can be referenced anywhere in the input by placing an "&" immediately preceding the parameter name. If a minus sign “-“ is placed directly before “&”, i.e., “-&”, with no space the sign of the numerical value will be switched. 2. LOCAL Option. *PARAMETER_LOCAL behaves like the *PARAMETER keyword with one difference. A parameter defined by *PARAMETER without the LOCAL option is visible and available at any later point in the input pro- cessing. Parameters defined via the LOCAL versions disappear when the input parser finishes reading the file in which they appear. LOCAL variables can temporarily mask non-LOCAL variables. For example, suppose you have the following input files: main.k: *PARAMETER R VAL1 1.0 *PARAMETER R VAL2 2.0 *PARAMETER R VAL3 3.0 *CONTROL_TERMINATION &VAL1 *INCLUDE file1 file1: *PARAMETER R VAL1 10.0 *PARAMETER_LOCAL R VAL2 20.0 *PARAMETER_LOCAL R VAL4 40.0 *INCLUDE file2 ⋮ Then, inside file2 we will see VAL1 = 10.0, VAL2 = 20.0, VAL3 = 3.0 and VAL4 = 40.0. In main.k, after returning from file1, we will see VAL1 = 10.0, VAL2 = 2.0, and VAL3 = 3.0. VAL4 will not exist. This allows for include files that can set all their own parameters without clobbering the parameters in the rest of the input. 3. MUTABLE Option for Redefining. The MUTABLE option is used to indicate that an integer or real parameter may be redefined at some later point in the input processing (it is ignored for character parameters). Redefinition is al- lowed regardless of the setting of *PARAMETER_DUPLICATION. The MU- TABLE qualifier must appear on the first definition of the parameter. It is not required on any later redefinition. *PARAMETER Purpose: The purpose is to control how the code behaves if a duplicate parameter definition is found in the input. Card 1 1 2 3 4 5 6 7 8 Variable DFLAG Type Default I 1 VARIABLE DESCRIPTION DFLAG Flag to control treatment of duplicate parameter definitions: EQ.1: issue a warning and ignore the new definition (default) EQ.2: issue a warning and accept the new definition EQ.3: issue an error and ignore (terminates at end of input) EQ.4: accept silently EQ.5: ignore silently Remarks: A LOCAL variable appearing in a file, which masks a non-LOCAL parameter, won't trigger these actions; however, a LOCAL that masks another LOCAL or a non-LOCAL that masks a non-LOCAL will Only one *PARAMETER_DUPLICATION card is allowed. If more than one is found, a warning is issued and any after the first are ignored. *PARAMETER_EXPRESSION_{OPTION} The available options are <BLANK> LOCAL MUTABLE Purpose: Define the numerical values of parameter names referenced throughout the input file. Like the *PARAMETER keyword, but allows for general algebraic expressions, not simply fixed values. The LOCAL option allows for include files to contain their own unique expressions without clobbering the expressions in the rest of the input. See the *PARAMETER keyword. Parameter Cards. Include as many cards as necessary. Card 1 1 2 3 4 5 6 7 8 Variable PRMR1 EXPRESSION1 Type A Default none VARIABLE PRMRn A none DESCRIPTION Define the nth parameter in a field of 10. Within this field the first character must be either an "R" for a real number, "I" for an integer, or “C” for a character string. Lower or upper case for "I/C/R" is okay. Following the type designation, define the name of the parameter using up to, but not exceeding nine characters. For example, when defining a shell thickness named, "SHLTHK", both inputs "RSHLTHK" or "R SHLTHK" can be used and placed anywhere in the field of 10. When referencing SHLTHK in the input file see Remark 1 below. EXPRESSIONn General expression which is evaluated, having the result stored in PRMRn. The following functions are available: sin, cos, tan, csc, sec, ctn, asin, acos, atan, atan2, sinh, cosh, tanh, asinh, acosh, atanh, min, max, sqrt, mod, abs, sign, int, aint, nint, anint, float, exp, log, log10, float, pi, and general arithmetic expressions involving +, -, *, /, and **. VARIABLE DESCRIPTION The standard rules regarding operator precedence are obeyed, and nested parentheses are allowed. The expression can reference previously defined parameters (with or without the leading &). The expression can be continued on multiple lines simply by leaving the first 10 characters of the continuation line blank. For type “C” parameters, the expression is not evaluated in any sense, just stored as a string. Remarks: 1. Parameters can be referenced anywhere in the input by placing an "&" immediately preceding the parameter name. Expressions can be included in the input when placed between brackets “<>” as long as the total line length does not exceed 80 columns and fields are comma-delimited. For example, this… *parameter rterm, 0.2, istates, 80 *parameter_expression rplot,term/(states-30) *DATABASE_BINARY_D3PLOT &plot is equivalent to *parameter rterm, 0.2, istates, 80 *DATABASE_BINARY_D3PLOT <term/(states-30)>, 2. The integer and real properties of constants and parameters are honored when evaluating expressions. So 2/5 becomes 0, but 2.0/5 becomes 0.4. 3. The sign, atan2, min, max, and mod functions all take two arguments. The others all take only 1. 4. Functions that use an angle as their argument, e.g., sin or cos, assume the angle is in radians. 5. The MUTABLE option is used to indicate that an integer or real parameter may be redefined at some later point in the input processing (it is ignored for charac- Redefinition is allowed regardless of the setting of ter parameters). *PARAMETER_DUPLICATION. The MUTABLE qualifier must appear on the first definition of the parameter. It is not required on any later redefinition. 6. The unary minus has higher precedence than exponentiation, i.e. the formula - 3**2 will be interpreted as (−3)2 = 9. *PARAMETER *PARAMETER_TYPE is a variation on the *PARAMETER keyword command. In addition to its basic function of associating a parameter name (PRMR) with a numerical value (VAL), the *PARAMETER_TYPE command also includes information (PRTYP) about how the parameter is used by LS-DYNA, e.g., as a Part ID or as a segment set ID. *PARAMETER_TYPE is useful only when (1) the parameter is used to represent an integer ID number, and (2) LS-PrePost is used to combine two or more models (keyword decks) into a larger model. Only by knowing how the parameter is used by LS-DYNA is LS-PrePost able to increment the parameter value by the proper “offset” when LS-PrePost combines two or more input decks together into a larger deck. These offsets are necessary so that IDs of a certain type, e.g., Part IDs, are not duplicated in the assembled model. Figure 30-1 (b) shows the offset input dialog box of LS-PrePost where offset values for specific ID types are assigned. Background: This command is designed to support workflows involving models that are built up from discrete subassemblies created by independent workgroups. As the subassembly models evolve through the design process, Part IDs, material IDs, etc. in the models may change with each design iteration and therefore it is advantageous to parameterize those IDs. In this way, though the parameter values may change, the parameter names remain the same. When the subassembly models are combined by LS-PrePost to create a larger model of an assembly or of a complete system, for instance, an aircraft engine model, parameter values assigned using *PARAMETER_TYPE are incremented by the proper ID offset value as prescribed when LS-PrePost imports each keyword file. *PARAMETER_TYPE Parameter Cards. For each parameter with type information, include an additional card. This input ends at the next keyword (“*”) card. Card 1 1 2 3 4 5 6 7 8 Variable PRMR VAL PRTYP Type A I A Default none None none Subsystem ID: 3, Name: Filename: Browse Offset Settings Import Offset Import No Offset Cancel (a) Import With Offset Default Offset Set Largest ID NODE PART SECTION DEFINE_COORD SET_DISCRETE SET_PART SET_SHELL SET_TSHELL ELEMENT/S/STRAIN MAT DEFINE_CURVE SET_BEAM SET_NODE SET_SEGMENT SET_SOLID EOS More... Import Cancel (b) Figure 30-1. (a) the file → import → keyword dialog box; (b) the LS-PrePost dialog that takes the offset as a function of ID type. VARIABLE DESCRIPTION PRMR PRMR must be in the following format PRMR = I xxxxxxxxx ⏟⏟⏟⏟⏟⏟⏟ 9 character name The first character is the type indicator and must be set to “I” for integer. The remaining 9 characters specifiy the name of the parameter. input For example, to define a part ID "WHLPID", the “IWHLPID”, “I␣␣␣WHLPID”, or “I␣␣WHLPID␣” are all equivalent 10 character strings (“␣” is space). For instructions regard how to use the variable “WHLPID” see remark 1. VAL Define the value of the parameter. The VAL field must contain an integer. VARIABLE PRTYP DESCRIPTION Describes, for the benefit of LS-PrePost only, how the parameter PRMR is used by LS-DYNA. PRTYP is ignored by LS-DYNA. For example, if VAL represents a Part ID, then PRTYP should be set to “PID”. Knowing how the parameter is used by LS-DYNA, LS-PrePost can apply the appropriate offset to VAL when input decks are combined using LS-PrePost. EQ.NID: EQ.NSID: EQ.PID: EQ.PSID: EQ.MID: Node ID, Node set ID, Part ID, Part set ID, Material ID, EQ.EOSID: Equation of state ID, EQ.BEAMID: Beam element ID, EQ.BEAMSID: Beam element set ID, EQ.SHELLID: Shell element ID, EQ.SHELLSID: Shell element set ID, EQ.SOLIDID: Solid element ID, EQ.SOLIDSID: Solid element set ID, EQ.TSHELLID: Tshell element ID, EQ.TSHELLSID: Tshell element set ID, EQ.SSID: Segment set ID Remarks: 1. Parameters can be referenced anywhere in the input by placing an "&" at the first column of its field followed by the name of the parameter without blanks. For example if PRMR is set to “I␣␣WHLPID␣” then the appropriate reference is “&WHLPID”. Example: *PARAMETER_TYPE I WHLPID 100 PID I WHLMID 300 MID *PART Wheel &WHLPID,200,&WHLMID 2. *PARAMETER_TYPE is only supported by LS-PrePost 4.1 or later. 3. Combining *INCLUDE_TRANSFORM with *PARAMETER_TYPE is unsup- ported. This will introduce conflicting parameter offset values, and offset val- ues specified in *INCLUDE_TRANSFORM will override offset values associated with *PARAMETER_TYPE. The following keywords are used in this section: *PART_{OPTION1}_{OPTION2}_{OPTION3}_{OPTION4}_{OPTION5} *PART_ADAPTIVE_FAILURE *PART_ANNEAL *PART_COMPOSITE_{OPTION} *PART_DUPLICATE *PART_MODES *PART_MOVE *PART_SENSOR *PART_STACKED_ELEMENTS *PART_{OPTION1}_{OPTION2}_{OPTION3}_{OPTION4}_{OPTION5} For OPTION1 the available options are <BLANK> INERTIA REPOSITION For OPTION2 the available options are <BLANK> CONTACT For OPTION3 the available options are <BLANK> PRINT For OPTION4 the available options are <BLANK> ATTACHMENT_NODES For OPTION5 the available options are <BLANK> AVERAGED Options 1, 2, 3, 4, and 5 may be specified in any order on the *PART card. Purpose: Define parts, i.e., combine material information, section properties, hourglass type, thermal properties, and a flag for part adaptivity. The INERTIA option allows the inertial properties and initial conditions to be defined rather than calculated from the finite element mesh. This applies to rigid bodies, see *MAT_RIGID, only. The REPOSITION option applies to deformable materials and is used to reposition deformable materials attached to rigid dummy components whose motion is controlled by either CAL3D or MADYMO. At the beginning of the is automatically calculation each component controlled by CAL3D/MADYMO repositioned to be consistent with the CAL3D/MADYMO input. However, deformable materials attached to these components will not be repositioned unless this option is used. The CONTACT option allows part based contact parameters to be used with the automatic contact types a3, 4, a5, b5, a10, 13, a13, 15 and 26, that is *CONTACT_AUTOMATIC_SURFACE_TO_SURFACE, *CONTACT_AUTOMATIC_SURFACE_TO_SURFACE_MORTAR, *CONTACT_SINGLE_SURFACE, *CONTACT_AUTOMATIC_NODES_TO_SURFACE, *CONTACT_AUTOMATIC_BEAMS_TO_SURFACE, *CONTACT_AUTOMATIC_ONE_WAY_SURFACE_TO_SURFACE, *CONTACT_AUTOMATIC_SINGLE_SURFACE, *CONTACT_AUTOMATIC_SINGLE_SURFACE_MORTAR, *CONTACT_AIRBAG_SINGLE_SURFACE, *CONTACT_ERODING_SINGLE_SURFACE, *CONTACT_AUTOMATIC_GENERAL. The default values to use for these contact parameters can be specified on the *CONTACT input section card. The PRINT option allows user control over whether output data is written into the ASCII files MATSUM and RBDOUT. See *DATABASE_ASCII. The AVERAGED option may be applied only to parts consisting of a single (non- branching) line of truss elements. The average strain and strain rate over the length of the truss elements in the part is calculated, and the resulting average axial force is applied to all of the elements in the part. Truss elements in an averaged part form one long continuous “macro-element.” The time step size for an AVERAGED part is based on the total length of the assembled trusses, rather than on the shortest truss. Effectively, the truss elements of an AVERAGED part behave as a string under uniform tension. In an AVERAGED part there are no internal forces acting to keep the nodes separated, and other force contributions from the surrounding system must play that role. Therefore, the nodes connected to the truss elements should be attached to other structural members. This model is prototypically used for modeling cables in mechanical actuators. The AVERAGED option can be activated for all material types, which are available for truss elements. Card Sets. Repeat as many sets data cards as desired (card 1 through 10). This input ends at the next keyword (“*”) card. Card 1 1 2 3 4 5 6 7 8 Variable Type Default HEADING C none Card 2 1 2 3 4 5 6 7 8 Variable PID SECID MID EOSID HGID GRAV ADPOPT TMID Type I/A I or A10 I or A10 I or A10 I or A10 Default none none none 0 0 I 0 I 0 I or A10 0 Inertia Card 1. Additional Card for the INERTIA option. See Remarks 2, 3, and 4. Card 3 Variable 1 XC Type F 2 YC F 3 ZC F 4 TM 5 6 7 8 IRCS NODEID F I I Inertia Card 2. Additional Card for the INERTIA option. Card 4 1 Variable IXX 2 IXY 3 IXZ 4 IYY 5 IYZ 6 IZZ 7 8 Type F F F F F Inertia Card 3. Additional Card for the INERTIA option. Card 5 1 2 3 4 5 6 7 8 Variable VTX VTY VTZ VRX VRY VRZ Type F F F F F F Inertial Coordinate System Card. Optional card required for IRCS = 1 with INERTIA option. Define two local vectors or a local coordinate system ID. Card 6 Variable Type Remark 1 XL F 1 2 YL F 1 3 ZL F 1 4 5 6 7 8 XLIP YLIP ZLIP CID F 1 F 1 F 1 I none Reposition Card. An additional Card is for the REPOSITION option. Card 7 1 2 3 4 5 6 7 8 Variable CMSN MDEP MOVOPT Type I I I Contact Card. Additional Card is required for the CONTACT option. Card 8 Variable 1 FS Type F 2 FD F 3 DC F 4 VC F 5 6 7 8 OPTT SFT SSF CPARM8 F F F NOTE: If FS, FD, DC, and VC are specified they will not be used unless FS is set to a negative value (-1.0) in the *CONTACT section. These frictional coefficients apply only to contact types: SINGLE_SURFACE, AUTOMATIC_GENERAL, AUTOMATIC_SINGLE_SURFACE, AUTOMATIC_SINGLE_SURFACE_MORTAR, AUTOMATIC_NODES_TO_..., AUTOMATIC_SURFACE_..., AUTOMATIC_SURFACE_..._MORTAR, AUTOMATIC_ONE_WAY_..., ERODING_SINGLE_SURFACE Default values are input via *CONTROL_CONTACT input. Print Card. An additional Card is required for the PRINT option. This option applies to rigid bodies and provides a way to turn off ASCII output in files rbdout and matsum. Card 9 1 2 3 4 5 6 7 8 Variable PRBF Type I Attachment Nodes Card. Additional Card required for the ATTACHMENT_NODES option. See Remark 8. Card 10 1 2 3 4 5 6 7 8 Variable ANSID Type I VARIABLE DESCRIPTION HEADING Heading for the part PID Part identification. A unique number or label must be specified. VARIABLE DESCRIPTION SECID MID EOSID HGID Section See Remark 7. identification defined in a *SECTION keyword. Material See Remark 7. identification defined in the *MAT section. Equation of state identification defined in the *EOS section. Nonzero only for solid elements using an equation of state to compute pressure. See Remark 7. Hourglass/bulk viscosity identification defined in the *HOUR- GLASS Section. See Remark 7. EQ.0: default values are used. GRAV Flag to turn on gravity initialization according to *LOAD_DENSI- TY_DEPTH. EQ.0: Part will be initialized only if included in the part set PSID in *LOAD_DENSITY_DEPTH. EQ.1: Part will be initialized irrespective of PSID in *LOAD_ DENSITY_DEPTH. ADPOPT Indicate if this part is adapted or not. : LT.0: 𝑟-adaptive remeshing for 2-D solids, |ADOPT| gives the load curve ID that defines the element size as a function of time. EQ.0: Adaptive remeshing is inactive for this part ID. EQ.1: ℎ-adaptive for 3-D shells. EQ.2: 𝑟-adaptive remeshing for 2-D solids, 3-D tetrahedrons and 3-D EFG. EQ.3: Axisymmetric r-adaptive remeshing for 3-D solid . EQ.9: Passive ℎ-adaptive for 3-D shells. The elements in this part will not be split unless their neighboring elements in other parts need to be split more than one level. TMID *PART DESCRIPTION Thermal material property identification defined in the *MAT_- THERMAL Section. Thermal properties must be specified for all solid, shell, and thick shell parts if a thermal or coupled thermal structural/analysis is being performed. Discrete elements are not considered in thermal analyses. See Remark 7. XC YC ZC TM Global 𝑥-coordinate of center of mass. If nodal point, NODEID, is defined XC, YC, and ZC are ignored and the coordinates of the nodal point, NODEID, are taken as the center of mass. Global 𝑦-coordinate of center of mass Global 𝑧-coordinate of center of mass Translational mass IRCS Flag for inertia tensor reference coordinate system: EQ.0: global inertia tensor, EQ.1: local inertia tensor is given in a system defined by the orientation vectors. NODEID Nodal point defining the CG of the rigid body. This node should be included as an extra node for the rigid body; however, this is not a requirement. If this node is free, its motion will not be updated to correspond with the rigid body after the calculation begins. IXX IXY IXZ IYY IYZ IZZ VTX 𝐼𝑥𝑥, 𝑥𝑥 component of inertia tensor 𝐼𝑥𝑦,, 𝑥𝑦 component of inertia tensor 𝐼𝑥𝑧, 𝑥𝑧 component of inertia tensor 𝐼𝑦𝑦, 𝑦𝑦 component of inertia tensor 𝐼𝑦𝑧, 𝑦𝑧 component of inertia tensor 𝐼𝑧𝑧, 𝑧𝑧 component of inertia tensor initial translational velocity of rigid body in global 𝑥 direction VARIABLE DESCRIPTION VTY VTZ VRX VRY VRZ XL YL ZL XLIP YLIP ZLIP CID initial translational velocity of rigid body in global 𝑦 direction initial translational velocity of rigid body in global 𝑧 direction initial rotational velocity of rigid body about global 𝑥 axis initial rotational velocity of rigid body about global 𝑦 axis initial rotational velocity of rigid body about global 𝑧 axis 𝑥-coordinate of local 𝑥-axis. Origin lies at (0, 0, 0). 𝑦-coordinate of local 𝑥-axis 𝑧-coordinate of local 𝑥-axis 𝑥-coordinate of vector in local 𝑥-𝑦 plane 𝑦-coordinate of vector in local 𝑥-𝑦 plane 𝑧-coordinate of vector in local 𝑥-𝑦 plane Local coordinate system ID, see *DEFINE_COORDINATE_… With this option leave fields 1 - 6 blank. CMSN CAL3D segment number / MADYMO system number. See the numbering in the corresponding program. MDEP MADYMO ellipse/plane number: GT.0: ellipse number, EQ.0: default, LT.0: absolute value is plane number. MOVOPT FS FD DC VC *PART DESCRIPTION Flag to deactivate moving for merged rigid bodies, see *CON- STRAINED_RIGID_BODIES. This option allows a merged rigid body to be fixed in space while the nodes and elements of the generated CAL3D/MADYMO parts are repositioned: EQ.0: merged rigid body is repositioned, EQ.1: merged rigid body is not repositioned. Static coefficient of friction. The functional coefficient is assumed to be dependent on the relative velocity 𝑣relof the surfaces in contact, 𝜇𝑐 = FD + (FS − FD)𝑒−DC×∣𝑣rel∣. For mortar contact 𝜇𝑐 = FS, i.e., dynamic effects are ignored. Dynamic coefficient of friction. The functional coefficient is assumed to be dependent on the relative velocity 𝑣rel of the surfaces in contact 𝜇𝑐 = FD + (FS − FD)𝑒−DC×∣𝑣𝑟𝑒𝑙∣. For mortar contact 𝜇𝑐 = FS, i.e., dynamic effects are ignored. Exponential decay coefficient. The functional coefficient is assumed to be dependent on the relative velocity vrel of the surfaces in contact 𝜇𝑐 = FD + ( FS − FD)𝑒−DC×∣𝑣rel∣. For mortar contact 𝜇𝑐 = FS (dynamical effects are ignored). Coefficient for viscous friction. This is necessary to limit the friction force to a maximum. A limiting force is computed by, 𝐹lim = VC × 𝐴cont, where 𝐴cont is the area of the segment contacted by the node in contact. The suggested value for VC is to use the yield stress in shear VC = where 𝜎0 is the yield stress of the contacted 𝜎𝑜 √3 material. OPTT Optional contact thickness. This applies to solids, shells and beams. VARIABLE DESCRIPTION SFT SSF Optional thickness scale factor for PART ID in automatic contact (scales true thickness). This option applies only to contact with shell elements. True thickness is the element thickness of the shell elements. Scale factor on default slave penalty stiffness for this PART ID whenever it appears in the contact definition. If zero, SSF is taken as unity. CPARM8 Flag to exclude beam-to-beam contact from the same PID for CONTACT_AUTOMATIC_GENERAL. This applies only to MPP. Global default may be set using CPARM8 on *CON- TACT_…_MPP Optional Card. EQ.0: Flag is not set (default). EQ.1: Flag is set. EQ.2: Flag is set. CPARM8 = 2 has the additional effect of permitting contact treatment of spot weld (type 9) beams in AUTOMATIC_GENERAL contacts; spot weld beams are otherwise disregarded entirely by AUTOMATIC_- GENERAL contacts. PRBF Print flag for rbdout and matsum files. EQ.0: default is taken from the keyword *CONTROL_OUT- PUT. EQ.1: write data into rbdout file only EQ.2: write data into matsum file only EQ.3: do not write data into rbdout and matsum Attachment node set ID. See Remark 8. This option should be used very cautiously and applies only to rigid bodies. The attachment point nodes are updated each cycle whereas other nodes in the rigid body are updated only in the output databases. All loads seen by the rigid body must be applied through this nodal subset or directly to the center of gravity of the rigid body. If the rigid body is in contact this set must include all interacting nodes. EQ.0: All nodal updates are skipped for this rigid body. The null option can be used if the rigid body is fixed in space or if the rigid body does not interact with other parts, e.g., the rigid body is only used for some visual purpose. *PART VARIABLE ANSID Remarks: 1. Local Inertia Tensor Coordinate System. The local Cartesian coordinate system is defined as described in *DEFINE_COORDINATE_VECTOR. The local 𝑧-axis vector is the vector cross product of the 𝑥-axis and the in-plane vector. The local 𝑦-axis vector is finally computed as the vector cross product of the 𝑧-axis vector and the 𝑥-axis vector. The local coordinate system defined by CID has the advantage that the local system can be defined by nodes in the rigid body which makes repositioning of the rigid body in a preprocessor much easier since the local system moves with the nodal points. 2. 3. 4. Inertia Option and Shared Rigid/Deformable Nodes. When specifying mass properties for a rigid body using the inertia option, the mass contributions of deformable bodies to nodes which are shared by the rigid body should be con- sidered as part of the rigid body. Inertia Option Lacks Default Values. If the inertia option is used, all mass and inertia properties of the body must be specified. There are no default values. Inertia Tensor Characteristics. The inertia terms are always with respect to the center of mass of the rigid body. The reference coordinate system defines the orientation of the axes, not the origin. Note that the off-diagonal terms of the inertia tensor are opposite in sign from the products of inertia. 5. Initial Velocity Card for Rigid Bodies. The initial velocity of the rigid body may be overwritten by the *INITIAL_VELOCITY card. 6. Axisymmetric Remeshing. Axisymmetric remeshing is specially for 3-D orbital forming. The adaptive part using this option needs to meet the follow- ing requirement in both geometry and discretization: a) The geometry is (quasi-) symmetric with respect to the local 𝑧-axis, which in turn must be parallel to the global 𝑧-axis. See CID in *CONTROL_- REMESHING. b) A set of 2-D cross-sections with uniform angular interval around 𝑧-axis are discretized by mixed triangular and quadrilateral elements in a similar pattern. c) A set of circular lines around 𝑧-axis pass through the nodes of the cross- sections and form orbital pentahedrons and hexahedrons. 7. Allowed ID Values. The variables SID, MID, EOSID, HGID, and TMID in *PART, and in *SECTION, *MAT, *EOS, *HOURGLASS, and *MAT_THER- MAL, respectively, may be input as an 10-character alphanumeric variable (20- characters if long format is used), e.g., “HS Steel”, or as an integer not to exceed 232 − 1, e.g.,“123456789” is allowed. 8. Attachment Nodes Option. All nodes are treated as attachment nodes if this option is not used. Attachment nodes apply to rigid bodies only. The motion of these nodes, which must belong to the rigid body, are updated each cycle. Other nodes in the rigid body are updated only for output purposes. Include all nodes in the attachment node set which interact with the structure through joints, contact, merged nodes, applied nodal point loads, and applied pressure. Include all nodes in the attachment node set if their displacements, accelera- tions, and velocities are to be written into an ASCII output file. Body force loads are applied to the c.g. of the rigid body. *PART_ADAPTIVE_FAILURE Purpose: This is an option for two-dimensional adaptivity to allow a part that is singly connected to split into two parts. This option is under development and will be generalized in the future to allow the splitting of parts that are multiply connected. 3 4 5 6 7 8 Card 1 1 Variable PID Type I 2 T F VARIABLE DESCRIPTION PID T Part ID Thickness. When the thickness of the part reaches this minimum value the part is split into two parts. The value for T should be on the order of the element thickness of a typical element. Available options include: <BLANK> SET *PART Purpose: To initialize the stress states at integration points within a specified part to zero at a given time during the calculation. This option is valid for parts that use constitutive models where the stress is incrementally updated. This option applies to the Hughes-Liu beam elements, the integrated shell elements, thick shell elements, and solid elements. In addition to the stress tensor components, the effective plastic strain is also set to zero. Part Cards. Include as many parts cards as desired. This input ends at the next keyword (“*”) card. Card 1 1 2 3 4 5 6 7 8 Variable PID/PSID TIME Type I F Default none none VARIABLE DESCRIPTION PID/PSID Part ID or part set ID if the SET option is active. TIME Time when the stress states are reinitialized. *PART_COMPOSITE_{OPTION} Available options include: <BLANK> CONTACT TSHELL LONG Purpose: The following input provides a simplified method of defining a composite material model for shell elements and thick shell elements that eliminates the need for user defined integration rules and part ID’s for each composite layer. When *PART_- COMPOSITE is used, a section definition, *SECTION_SHELL or *SECTION_TSHELL, and integration rule definition, *INTEGRATION_SHELL, are unnecessary. The material ID, thickness, material angle and thermal material ID for each through- thickness integration point of a composite shell or thick shell are provided in the input for this command. The total number of integration points is determined by the number of entries on these cards. Unless the *ELEMENT_SHELL_THICKNESS card is set, the thickness is assumed to be constant on each shell element. The thickness, then, is given by summing the THICK𝑖 values from card 4 below over the integration points 𝑖. When the *ELEMENT_SHELL_- THICKNESS card is included the THICK𝑖 values are scaled to fit the nodal thickness values assigned using the *ELEMENT__SHELL_THICKNESS keyword. For thick shells, the total thickness is obtained from the positions of the nodes on the top and bottom surfaces. In this case, the THICKi, are also scaled to conform to the geometry defined by the element’s nodes. For a more general method of defining composite shells and thick shells, see *ELE- MENT_SHELL_COMPOSITE These commands permit unique layer stack-ups for each element without requiring a unique part ID for each element. *ELEMENT_TSHELL_COMPOSITE. and With *PART_COMPOSITE, two integration points with 4 constants each are provided in each Integration Point Properties Card. On the other hand, with *PART_COMPOS- ITE_LONG, for each integration point there is one Integration Point Properties Card containing up to 8 constants. To maintain a direct association of through-thickness integration point numbers with physical plies in the case where plies span over more than one part ID, see Remark 5. The CONTACT option allows part based contact parameters to be used with the automatic contact types a3, 4, a5, a10, 13, a13, 15 and 26, which are listed under the *PART definition above. Card Sets. Repeat as many sets data cards as desired. This input ends at the next keyword (“*”) card. Card 1 1 2 3 4 5 6 7 8 Variable Type Default HEADING C none Thin Shell Card. The following card is required for thin shell composites. Omit this card if the TSHELL option is used. Card 2 1 2 3 4 5 6 7 8 Variable PID ELFORM SHRF NLOC MAREA HGID ADPOPT THSHEL Type I Default none I 0 F F F 1.0 0.0 0.0 I 0 I 0 I 0 Thick Shell Card. This is an additional card for the TSHELL option. Card 2 1 2 3 4 5 6 7 8 Variable PID ELFORM SHRF HGID TSHEAR Type I Default none I 0 F 1.0 I 0 I Contact Card. Additional Card is required for the CONTACT option. Card 3 Variable 1 FS Type F 2 FD F 3 DC F 4 VC F 5 6 7 8 OPTT SFT SSF F F F NOTE: If FS, FD, DC, and VC are specified they will not be used unless FS is set to a negative value (-1.0) in the *CONTACT section. These frictional coefficients apply only to contact types: SINGLE_SURFACE, AUTOMATIC_GENERAL, AUTOMATIC_SINGLE_SURFACE, AUTOMATIC_NODES_TO_..., AUTOMATIC_SURFACE_..., AUTOMATIC_ONE_WAY_..., ERODING_SINGLE_SURFACE Default values are input via *CONTROL_CONTACT input. Integration Point Data Cards without Long Option. The material ID, thickness, and material angle for each through-thickness integration point of a composite shell are provided below (up to two integration points per card). The integration point data should be given sequentially starting with the bottommost integration point. The total number of integration points is determined by the number of entries on these cards. Include as many cards as necessary. The next “*” card terminates this input. Card 4 1 2 Variable MID1 THICK1 Type I F 3 B1 F 4 5 6 TMID1 MID2 THICK2 I I F 7 B2 F 8 TMID2 Integration Point Data Cards for Long Option. The material ID, thickness, and material angle for each through-thickness integration point of a composite shell are provided below (one integration point per card). The integration point data should be given sequentially starting with the bottommost integration point. The total number of integration points is determined by the number of entries on these cards. Include as many cards as necessary. The next “*” card terminates this input. Card 4 1 2 Variable MID1 THICK1 Type I F 3 B1 F 4 5 6 7 8 TMID1 PLYID1 SHRFAC I I F VARIABLE DESCRIPTION HEADING Heading for the part PID Part ID ELFORM Element formulation options for thin shells: EQ.1: Hughes-Liu, EQ.2: Belytschko-Tsay, EQ.3: BCIZ triangular shell, EQ.4: C0 triangular shell, EQ.6: S/R Hughes-Liu, EQ.7: S/R co-rotational Hughes-Liu, EQ.8: Belytschko-Leviathan shell, EQ.9: Fully integrated Belytschko-Tsay membrane, EQ.10: Belytschko-Wong-Chiang, EQ.11: Fast (co-rotational) Hughes-Liu, EQ.16: Fully integrated shell element (very fast), Element formulation options for thick shells: EQ.1: one point reduced integration, EQ.2: selective reduced 2 x 2 in plane integration, EQ.3: assumed strain 2 x 2 in plane integration, SHRF NLOC *PART_COMPOSITE DESCRIPTION EQ.5: assumed strain reduced integration with brick materials EQ.6: : assumed strain reduced integration with shell materials EQ.7: assumed strain 2x2 in plane integration Shear correction factor which scales the transverse shear stress. Location of reference surface, available for thin shells only. If nonzero, the offset distance from the plane of the nodal points to the reference surface of the shell in the direction of the shell normal vector is a value: offset = −0.50 × NLOC × (average shell thickness). This offset is not considered in the contact subroutines unless CNTCO is set to 1 in *CONTROL_SHELL. Alternatively, the offset can be specified by using the OFFSET option in the *ELE- MENT_SHELL input section. EQ.1.0: top surface, EQ.0.0: mid-surface (default), EQ.-1.0: bottom surface. MAREA Non-structural mass per unit area. This is additional mass which comes from materials such as carpeting. This mass is not directly included in the time step calculation. HGID Hourglass/bulk viscosity identification defined in the *HOUR- GLASS Section: EQ.0: default values are used. ADPOPT Indicate if this part is adapted or not. Also see, *CONTROL_- ADAPTIVITY: EQ.0: no adaptivity, EQ.1: H-adaptive for 3-D thin shells. THSHEL Thermal shell formulation EQ.0: Default is governed by THSHEL on *CONTROL_SHELL EQ.1: Thick thermal shell EQ.2: Thin thermal shell VARIABLE DESCRIPTION TSHEAR Flag for transverse shear stress distribution : FS FD DC VC EQ.0: Parabolic, EQ.1: Constant through thickness. Static coefficient of friction. The functional coefficient is assumed to be dependent on the relative velocity vrel of the surfaces in contact as 𝜇𝑐 = FD + (FS − FD)𝑒−DC×∣𝑣rel∣. Dynamic coefficient of friction. The functional coefficient is assumed to be dependent on the relative velocity vrel of the surfaces in contact as 𝜇𝑐 = FD + (FS − FD)𝑒−DC×∣𝑣rel∣. Exponential decay coefficient. The functional coefficient is assumed to be dependent on the relative velocity vrel of the surfaces in contact as 𝜇𝑐 = FD + (FS − FD)𝑒−DC×∣𝑣rel∣. Coefficient for viscous friction. This is necessary to limit the friction force to a maximum. A limiting force is computed 𝐹lim = VC × 𝐴cont. Acont being the area of the segment contacted by the node in contact. The suggested value for VC is to use the where 𝜎0 is the yield stress of the yield stress in shear VC = 𝜎𝑜 √3 contacted material. OPTT Optional contact thickness. This applies to shells only. SFT SSF Optional thickness scale factor for PART ID in automatic contact (scales true thickness). This option applies only to contact with shell elements. True thickness is the element thickness of the shell elements. Scale factor on default slave penalty stiffness for this PART ID whenever it appears in the contact definition. If zero, SSF is taken as unity. MIDi Material ID of integration point I, see *MAT_… Section. THICKi Thickness of integration point i. Bi *PART_COMPOSITE DESCRIPTION Material angle of integration point i. This material angle applies only to material types 21, 22, 23, 33, 33_96, 34, 36, 40, 41-50, 54, 55, 58, 59, 103, 103_P, 104, 108, 116, 122, 133, 135, 135_PLC, 136, 157, 158, 190, 219, 226, 233, 234, 235, 242, and 243. TMIDi Thermal material ID of integration point i PLYIDi Ply ID of integration point i (for post-processing purposes) SHRFACi Trnansverse shear stress scale factor Remarks: 1. Orthotropic Materials. In cases where there is more than one orthotropic material model referenced by *PART_COMPOSITE, the orthotropic material orientation parameters (AOPT, BETA, and associated vectors) from the material model of the first orthotropic integration point apply to all the orthotropic inte- gration points. AOPT, BETA, etc. input for materials of subsequent integration points is ignored. Bi, not to be confused with BETA, is taken into account for each integration point. 2. SHRF Field and Zero Traction Condition. Thick shell formulations 1, 2, and 3, and all shell formulations with the exception of BCIZ and DK elements, are based on first order shear deformation theory that yields constant transverse shear strains which violates the condition of zero traction on the top and bot- tom surfaces of the shell. For these elements, setting SHRF=0.83333 will com- pensate for this error and result in the correct transverse shear deformation, so long as all layers have the same transverse stiffness. SHRF is not used by thick shell forms 3, 5, or 7 except for materials 33, 36, 133, 135, and 243. 3. Thick Shell 5 or 6 and Shear Stress. Thick shell formulation 5 and 6 will look to the TSHEAR parameter and use either a parabolic transverse shear stress distribution when TSHEAR=0, or a constant shear stress distribution when TSHEAR=1. The parabolic option is recommended when elements are used in a single layer to model a plate or beam. The constant option may be better when elements are stacked so there are two or more elements through the thickness. 4. Laminated Shear Stress Theory to Minimize Discontinuities. For compo- sites that have a transverse shear stiffness that varies by layer, laminated shell theory, activated by LAMSHT on *CONTROL_SHELL, will correct the trans- verse shear stress to minimize stress discontinuities between layers and at the bottom and top surfaces by imposing a parabolic transverse shear stress. SHRF should be set to the default value of 1.0 when the shear stress distribution is parabolic. If thick shells are stacked so that there is more than one element through the thickness of a plate or beam model, setting TSHEAR=1 will cause a constant shear stress distribution which may be more accurate than parabolic. The TSHEAR parameter is available for all thick shell forms when laminated shell theory is active. Alternatively, a scale factor can be defined for transverse shear stress in each layer of shell or thick shell composites using the SHRFAC parameter. The inputted SHRFAC values are normalized so that overall shear stiffness is unaffected by the distribution. Therefore, only the ratio of parame- ter values is significant. 5. Assignment of Zero Thickness to Integration Points. The ability to assign zero- thickness integration points in the stacking sequence allows the number of integration points to remain constant even as the number of physical plies var- ies from part to part and eases post-processing since a particular integration point corresponds to a physical ply. Such a capability is important when one or more of the physical plies are not continuous across a composite structure. To represent a missing ply in *PART_COMPOSITE, set THICKi to 0.0 for the corre- sponding integration point and additionally, either set MID=-1 or, if the LONG option is used, set PLYID to any nonzero value. To carry this concept a step further, in cases where the number of physical plies varies from element to element in a part, one can assign zero thickness to inte- gration points in exactly the same manner as described above but on an ele- ment-by-element basis using *ELEMENT_SHELL_COMPOSITE(_LONG) or *ELMENT_TSHELL_COMPOSITE. When postprocessing the results using LS-PrePost version 4.5, read both the keyword deck and d3plot database into the code and then select Option > N/A gray fringe. Then, when viewing fringe plots for a particular integration point (FriComp > IPt > intpt#), the element will be grayed out if the selected integra- tion point is missing (or has zero thickness) in that element. The available OPTION is NULL_OVERLAY *PART_DUPLICATE This option is used to generate null shells for contact. Purpose: To provide a method of duplicating parts or part sets without the need to use the *INCLUDE_TRANSFORM option. Duplication Cards. This format is used when the keyword option is left <BLANK>. Include as many of these cards as desired. This input ends at the next keyword (“*”) card. Card 1 1 2 3 4 5 6 7 8 Variable PTYPE TYPEID IDPOFF IDEOFF IDNOFF TRANID Type A I Default none none I 0 I 0 I 0 I 0 Null Duplication Cards. This format is used when the keyword option is set to NULL_OVERLAY. Include as many of these cards as desired. This input ends at the next keyword (“*”) card. Card 1 1 2 3 4 5 Variable PTYPE TYPEID IDPOFF IDEOFF DENSITY Type A I Default none none I 0 I 0 F 0 8 6 E F 0 7 PR F 0 VARIABLE PTYPE DESCRIPTION Set to “PART” to duplicate a single part or “PSET” to duplicate a part set. TYPEID ID of part or part set to be duplicated. VARIABLE DESCRIPTION IDPOFF ID offset of newly created parts. IDEOFF ID offset of newly created elements. IDNOFF ID offset of newly created nodes. TRANID ID of *DEFINE_TRANSFORMATION to transform the existing nodes in a part or part set. DENSITY Density. E PR Young’s modulus. Poisson’s ratio. Remarks: 1. All parts sharing common nodes have to be grouped in a *PART_SET and duplicated in a single *PART_DUPLICATE command so that the newly dupli- cated parts still share common nodes 2. The following elements which need a PART to complete their definition can be duplicated by using this command: *ELEMENT_SOLID, *ELEMENT_DIS- CRETE, *ELEMENT_SHELL, *ELEMENT_TSHELL, *ELEMET_BEAM and *EL- EMENT_SEATBELT. 3. This command only duplicates definition of nodes, elements and parts, not the associated constraints. For example, TC and RC defined in *NODE will not be passed to the newly created nodes. 4. When IDNOFF = IDPOFF = IDEOFF = 0, the existing part, or part set, will be transformed as per TRANID, no new node or elements will be created. 5. The NULL_OVERLAY option may be used to generate 3 and 4-node null shell elements from the 6- and 8-node quadratic elements for use in contact. No additional nodes are generated. *PART_MODES Purpose: Treat a part defined with *MAT_RIGID as a linearized flexible body (LFB) whereby deformations are calculated from mode shapes. Unlike superelements (*ELEMENT_DIRECT_MATRIX_INPUT), linearized flexible bodies are accurate for systems undergoing large displacements and large rotations. Currently, linearized flexible bodies cannot share nodes with other linearized flexible bodies or rigid bodies; however, interconnections to other linearized flexible bodies or to rigid bodies can use the penalty joint option. The linearized flexible bodies are not implemented with the Lagrange multiplier joint option . The deformations are modeled using the modes shapes obtained experimentally or in a finite element analysis, e.g., NASTRAN .pch file or a LS-DYNA d3eigv or d3mode file. These files may contain a combination of normal modes, constraint modes, and attachment modes. For stress recovery in linearized flexible bodies, use of linear element formulations is recommended. A lump mass matrix is assumed in the implementation. See also *CONTROL_RIGID. Card 1 1 2 3 4 5 6 7 8 Variable PID NMFB FORM ANSID FORMAT KMFLAG NUPDF SIGREC Type I Card 2 1 I 2 I 3 I 4 I 5 I 6 I 7 8 Variable Type Default FILENAME C none Kept Mode Cards. Additional card KMFLAG = 1. Use as many cards as necessary to specify the NMFB kept modes. After NMFB modes are defined no further input is expected. Card 3. 1 2 3 4 5 6 7 8 Variable MODE1 MODE2 MODE3 MODE4 MODE5 MODE6 MODE7 MODE8 Type I I I I I I I I Default none nont none nont none nont none nont Optional Modal Damping Cards. This input ends at the next keyword (“*”) card. Card 4 1 2 3 4 5 6 7 8 Variable MSTART MSTOP DAMPF Type I I F Default none none none VARIABLE DESCRIPTION PID Part identification. This part must be a rigid body. NMFB Number of kept modes in linearized flexible body. The number of modes in the file, FILENAME, must equal or exceed NMFB. If KMFLAG = 0 the first NMFB modes in the file are used. FORM Linearized flexible body formulation. See remark 5 below. EQ.0: exact EQ.1: fast EQ.3: general formulation (default) EQ.4: general formulation without rigid body mode orthogonalization. ANSID Attachment node set ID (optional). FORMAT Input format of modal information: *PART_MODES DESCRIPTION EQ.0: NASTRAN.pch file. EQ.1: (not supported) EQ.2: NASTRAN.pch file (LS-DYNA binary version). The binary version of this file is automatically created if a NASTRAN.pch file is read. The name of the binary file is the name of the NASTRAN.pch file but with ".bin" ap- pended. The binary file is smaller and can be read much faster. EQ.3: LS-DYNA d3eigv binary eigenvalue database . EQ.4: LS-DYNA d3mode binary constraint/attachment mode database . KMFLAG Kept mode flag. Selects method for identifying modes to keep. This flag is not supported for FORMAT = 4 (d3mode). EQ.0: the first NMFB modes in the file, FILENAME, are used. EQ.1: define NMFB kept modes with additional input. NUPDF Nodal update flag. If active, an attachment node set, ANSID, must be defined. EQ.0: all nodes of the rigid part are updated each cycle. EQ.1: only attachment nodes are fully updated. All nodes in the body are output based on the rigid body motion without the addition of the modal displacements. For maximum benefit an attachment node set can also be defined with the PART_ATTACHMENT_NODES op- tion. The same attachment node set ID should be used here. VARIABLE DESCRIPTION SIGREC Stress recovery flag. EQ.0: Do not recover stress. EQ.1: Recover stress. EQ.2: Recover stress and then set the recovery stress as initial stress when switching to a deformable body via *DE- FORMABLE_TO_RIGID_AUTOMATIC. (shell formula- tions 16, 18, 20, 21 and solid formulation 2). EQ.3: Recover stress based on shell formulation 21, and then set the recovery stress as initial stress for shell formula- tion 16 when switching to a deformable body via *DE- (shell FORMABLE_TO_RIGID_AUTOMATIC formulation 16 only). FILENAME The path and name of a file which contains the modes for this rigid body. MODEn Keep normal mode, MODEn. MSTART First mode for damping, (1 ≤ MSTART ≤ NMFB). MSTOP Last mode for damping, MSTOP, (1 ≤ MSTOP ≤ NMFB). All modes between MSTART and MSTOP inclusive are subject to the same modal damping coefficient, DAMPF. DAMPF Modal damping coefficient, 𝜁 . Remarks: 1. The format of the file which contains the normal modes follows the file formats of NASTRAN output for modal information. 2. The mode set typically combines both normal modes and attachment modes. The eigenvalues for the attachment modes are computed from the stiffness and mass matrices. 3. The part ID specified must be either a single rigid body or a master rigid body which can be made up of many rigid parts. 4. The modal damping is defined by the modal damping coefficient 𝜁 , where a value of 1.0 equals critical damping. For a one degree of freedom model sys- tem, the relationship between the damping and the damping coefficient is 𝑐 = 2𝜁 𝜔𝑛𝑚, where c is the damping, m is the mass, and 𝜔𝑛 is the natural fre- quency, √𝑘/𝑚. 5. There are four formulations. The first is a formulation that contains all the terms of the linearized flexible body equations, and its cost grows approximate- ly as the square of the number of modes. The second formulation ignores most of the second order terms appearing in the exact equations and its cost grows linearly with the number of modes. If the angular velocities are small and if the deflections are small with respect to the geometry of the system, the cost sav- ings of the second formulation may make it more attractive than the first meth- od. Please note that the first two formulations are only applicable when the modes are eigenmodes computed for the free-free problem, that is including the 6 rigid body modes. The third formulation, the default, is a more general formulation which allows more general mode shapes. It is strongly recommended that the default formulation be used. The fourth formulation does not orthogonalize the modes with respect to the rigid body modes, and may allow boundary condi- tions to be imposed more simply in some cases that the third formulation. *PART Purpose: Translate a part by an incremental displacement in either a local or a global coordinate system. This option currently applies to parts defined either by shell and solid elements. All nodal points of the given part ID are moved. Care must be observed since parts that share boundary nodes with the part being moved must also be moved to avoid severe mesh distortions – the variable IFSET can be used to handle the situation. Part/Part Set Move Cards. Include as many of following cards as desired. This input ends at the next keyword (“*”) cards. Card 1 1 2 3 4 5 6 7 8 9 10 Variable PID/PSID XMOV YMOV ZMOV CID IFSET Type I F Default none 0.0 F 0.0 F 0.0 I 0 I 0 VARIABLE DESCRIPTION PID/PSID Part or part set identification number. XMOV YMOV ZMOV CID Move shell/solid part ID, PID, in the x-direction by the incremental distance, XMOV. Move shell/solid part ID, PID, in the y-direction by the incremental distance, YMOV. Move shell/solid part ID, PID, in the z-direction by the incremental distance, ZMOV. Coordinate system ID to define incremental displacement in local coordinate system. All displacements, XMOV, YMOV, and ZMOV, are with respect to CID. EQ.0: global IFSET Indicate if part set ID (SID), is used in PID/SID definition. EQ.0: part ID (PID) is used EQ.1: part set ID (SID) is used. *PART_MOVE 1. A new variable IFSET is added to address the move of multiple parts that share common boundary nodes, e.g., in case of tailor-welded blanks. The new varia- ble allows for a part set to be move simultaneously. For example, keyword *SET_PART_LIST can be used to include all tailor welded blank part IDs and the resulting Part Set ID can be used in this keyword. 2. Draw beads can be modeled as beam elements and moved in the same distance and direction as either the die or punch, depending on the draw types. 3. A partial keyword input is provided below to automatically position all tools in a toggle draw of a decklid inner, with a tailor welded blank consisting of PID 1 and PID5, as shown in Figure 31-1. With the use of the keyword *CONTROL_- FORMING_AUTOPOSITION_PARAMETER_SET, the tailor-welded blank part set ID 1 is to be positioned in the global Z-direction on top of the lower die cavity (part set ID 4); the binder (part set ID 3) is to be positioned on top of the blank; and finally the upper punch (part set ID 2) is to be positioned on top of the blank. The three positioning distances for the blank, upper binder and upper punch are calculated and stored in variables &blnkmv, &upbinmv, and &uppunmv, respectively. The keyword *PART_MOVE, with IFSET of “1”, is responsible to actually move the three part sets, using the three corresponding positioning variables. It is noted that the AUTOPOSITION keyword is only applicable to shell elements. *PARAMETER R blnkmv 0.0 R upbinmv 0.0 R uppunmv 0.0 *SET_PART_LIST 1 1,5 *SET_PART_LIST 2 2 *SET_PART_LIST 3 3 *SET_PART_LIST 4 4 *CONTROL_FORMING_AUTOPOSITION_PARAMETER_SET $ PID/SID CID DIR MPID/MSID Position PREMOVE THICK PARORDER 1 3 4 1 1.5 blnkmv 3 3 1 1 1.5 upbinmv 2 3 1 1 1.5 uppunmv $---+----1----+----2----+----3----+----4----+----5----+----6----+----7----+--- -8 *PART_MOVE $ PID XMOV YMOV ZMOV CID IFSET 1 0.0 0.0 &blnkmv 1 3 0.0 0.0 &upbinmv 1 2 0.0 0.0 &uppunmv 1 PID 2 / PSID 2 Upper punch PID 3 / PSID 3 Upper binder PID 5 / PSID 1 Blank #2 Laser weld line PID 1 / PSID 1 Blank #1 PID 4 / PSID 4 Lower cavity Figure 31-1. A tailor welded blank is positioned in a decklid (toggle draw). Revision information: This IFSET feature is available starting in LS-DYNA Revision #62935. It is also implemented in all the applicable stamping processes in LS-PrePost4.0 Metal Forming Application eZ-Setup (http://ftp.lstc.com/anonymous/outgoing/lsprepost/4.0/metalforming/). *PART_SENSOR Purpose: Activate and deactivate parts, based on sensor defined in ELEMENT_SEAT- BELT_SENSOR. This option applies to discrete beam element only. Sensor Part Coupling Cards. Include as many of the following cards as desired. This input ends at the next keyword (“*”) card. Card 1 1 2 3 4 5 6 7 8 Variable PID SIDA ACTIVE Type Default I 0 I 0 I 0 VARIABLE DESCRIPTION PID SIDA ACTIVE Part ID, which is controlled by sensor Sensor ID to activate or deactivate part. Flag. If zero, the part is active from time zero until a signal is received by the part to deactivate. If one, the part is inactive from time zero and becomes active when a signal is received by the part to activate. The history variables for inactive parts are initialized at time zero. *PART Purpose: This keyword provides a method of defining a stacked element model for shell-like structures. These types of plane load-bearing components possess a thickness which is small compared to their other (in-plane) dimensions. Their physical properties vary in the thickness direction according to distinct layers. Application examples include sandwich plate systems, composite laminates, plywood, and laminated glass. With this keyword it is possible to discretize layered structures by an arbitrary sequence of shell and/or solid elements over the thickness. Whether a physical ply should be discretized by shell or solid elements depends on the individual thickness and other mechanical properties. Every single layer can consist of one shell element over the thickness or one or several solid elements over thickness. The stacked element mesh can either be provided directly or it be automatically generated by LS-DYNA itself. For automatic generation extrusion methods are used to determine the new node locations that characterize the out-of-plane geometry. Each layer gets its own predefined properties such as individual thickness, material characteristic, and element type. A more detailed description of this feature including a detailed description of the appropriate mesh generation procedure is given in Erhart [2015]. Card 1 1 2 3 4 5 6 7 8 Variable Type Default HEADING C none Card 2 1 2 3 4 5 6 7 8 Variable PIDREF NUMLAY ADPOPT Type I I Default none none I Layer Data Cards. The part ID, section ID, material ID, hourglass ID, thermal material ID, thickness, and number of through thickness solid elements for each layer i of a stacked element model are provided below. The layer data should be given sequentially starting with the bottommost layer. This card should be included NUMLAY times (one for each layer). The definitions in Card 3 replace the usual *PART cards. Card 3 1 Variable PIDi 2 SIDi 3 4 5 6 7 8 MIDi HGIDi TMIDi THKi NSLDi Type I I I Default none none none I 0 I 0 F I none none VARIABLE DESCRIPTION HEADING Heading for the part composition. PIDREF Part ID of reference shell element mesh. NUMLAY Number of layers. ADPOPT Indicate are *CONTROL_ADAPTIVE): if parts EQ.0: inactive adapted or not. (See also PIDi SIDi MIDi HGIDi TMIDi EQ.1: h-adaptive refinement Part identification. Section identification for layer i defined in a *SECTION keyword. Material identification for layer i defined in a *MAT keyword. Hourglass identification for layer i defined in a *HOURGLASS keyword. Thermal material identification for layer i defined in a *MAT_- THERMAL keyword. THKi Thickness of layer i. DESCRIPTION Number of through-thickness solid elements for layer i. VARIABLE NSLDi Remarks: 1. Provided vs. Automatically Generated Meshes. In general, there are two different options for this keyword: a) The user provides a finished mesh comprising stacked shell and/or solid elements and then combines the corresponding part IDs using this key- word. This mode does not require a reference mesh in the PIDREF field nor does it require that either the layer thickness (THKi fields) and the the number of through-thickness solids elements (NSLDi fields) be specfied. b) The user may provide a shell reference mesh (PIDREF) together with the layup sequence. The stacked element mesh is automatically generated during the initialization phase of LS-DYNA. In that second case, layer thickness (THKi) and number of through-thickness solids (NSLDi) must be defined. 2. Shell Solid Overlap. In the mesh generation case, two consecutive layers (solid-solid or solid-shell) are firmly connected, meaning that they share nodes in the most obvious way possible (except they are both shell element layers, see Remark 3 for that case). This condition leads to the necessity that shell and solid elements partly overlap if they follow each other in the stacking sequence. This deficiency can be corrected afterwards by subsequent relocation of the shell mid-surfaces via NLOC on *SECTION_SHELL (only works for first or last layer in this stacked element approach) or appropriate adjustment of the mate- rial stiffness for the solid elements. 3. Stacked Shells. Starting with the release of LS-DYNA version R10, it is possible to define shell element layers directly on top of each other (i.e. without solid elements in between). A potential connection/interaction of such layers has to be declared separately by additional contact definitions (standard, tied, or tiebreak) otherwise they are free to penetrate each other. 4. Chained Calculations. This keyword (*PART_STACKED_ELEMENTS) can also be used for modeling multi-stage processes. The *INTERFACE_SPRING- BACK_LSDYNA card can be used to save a final state including deformed geometry, stresses, and strains to a dynain file. In a subsequent calculation the *INCLUDE keyword can be used with that dynain to apply the layup sequence without regenerating the mesh. LS-DYNA automatically detects if a reference shell element mesh is present or not. 5. An Example. An example specifying a three layer shell-solid-shell structure is given below: *PART_STACKED_ELEMENTS $ title sandwich $ pidref numlay 11 3 $# pid sid mid hgid tmid thk nsld 100 200 1 1 0 0.25 0 101 201 2 0 0 0.60 3 102 200 1 1 0 0.15 0 *SECTION_SHELL $ sid elform shrf nip propt qr/irid 200 2 0.833 5.0 1.0 0.0 $ t1 t2 t3 t4 0.25 0.25 0.25 0.25 *SECTION_SOLID $ sid elform 201 -1 A sandwich structure is discretized by shell elements (SID = 200) on the outer layers with part identifiers 100 and 102. The interior of the “sandwich” consists of three solid elements (SID = 201, NSLD = 3) part identifier 101. In this case, the reference shell mesh belongs to part 11 (PIDREF). The thickness of each layer is defined by the value of the THK field, which will overwrite the thick- ness values from *SECTION_SHELL. Related materials (MID, TMID) and hourglass types (HGID) are treated as usual and therefore not shown here. *PARTICLE Purpose: To define control parameters for particle based blast loading. Card 1 1 2 3 4 5 6 7 8 Variable LAGSID LAGSTYPE NODID NODTYPE HECID HECTYPE AIRCID Type Default I 0 Card 2 1 I 0 2 I 0 3 I 0 4 I 0 5 I 0 6 I 0 7 8 Variable NPHE NPAIR IUNIT Type Default I 0 Card 3 1 I 0 2 I 0 3 4 5 6 7 8 Variable IHETYPE DENSITY ENERGY GAMMA COVOL DETO_V Type Default I 0 Card 4 1 F 0 2 F 0 3 F 0 4 F 0 5 F 0 6 Variable DETX DETY DETZ TDET BTEND NID Type Default F 0 F 0 F 0 F 0 F 0 I 0 7 Card 5 1 2 3 4 5 6 7 8 Variable BCX0 BCX1 BCY0 BCY1 BCZ0 BCZ1 Type Default F 0 Card 6 1 F 0 2 F 0 3 F 0 4 F 0 5 F 0 6 7 8 Variable IBCX0 IBCX1 IBCY0 IBCY1 IBCZ0 IBCZ1 BC_P Type Default I 0 I 0 I 0 I 0 I 0 I 0 I 0 VARIABLE DESCRIPTION LAGSID Structure id for particle structure interaction LAGSTYPE Structure type EQ.0: Part Set EQ.1: Part NODID Discrete element sphere (DES) or Smooth particle hydrodynamics (SPH) id for the interaction between particles and nodes. NODTYPE Nodal type EQ.0: Node Set EQ.1: Node EQ.2: Part Set EQ.3: Part HECID Initial container for high explosive particle VARIABLE DESCRIPTION HECTYPE Structure type EQ.0: Part Set EQ.1: Part EQ.2: Geometry, see *DEFINE_PBLAST_GEOMETRY AIRCID Initial geometry for air particles EQ.0: filled air particles to entire domain defined by Card 5 GT.0: Reference to *DEFINE_PBLAST_AIRGEO ID NPHE Number of high explosive particles NPAIR Number of air particles IUNIT Unit System EQ.0: Kg-mm-ms-K EQ.1: SI Units EQ.2: Ton-mm-s-K EQ.3: g-cm-us-K EQ.4: 𝑙𝑏𝑓 ∙ 𝑠2/𝑖𝑛- 𝑖𝑛 -s-K IHETYPE High Explosive type EQ.1: TNT EQ.2: C4 Others: Self Define DENSITY High Explosive density ENERGY High Explosive energy per unit volume GAMMA High Explosive fraction between 𝐶𝑝 and 𝐶𝑣 COVOL High Explosive co-volume DET_V High Explosive detonation velocity DETX DETY Detonation point 𝑥 Detonation point 𝑦 VARIABLE DESCRIPTION DETZ TDET Detonation point 𝑧 Detonation time BTEND Blast end time NID BCX0 BCX1 BCY0 BCY1 BCZ0 BCZ1 An optional node ID defining the position of the detonation point. If defined, its coordinates will overwrite the DETX, DETY, and DETZ defined above. Global domain 𝑥-min Global domain 𝑥-max Global domain 𝑦-min Global domain 𝑦-max Global domain 𝑧-min Global domain 𝑧-max IBCX0 Boundary conditions for global domain 𝑥-min EQ.0: Free EQ.1: Rigid reflecting boundary IBCX1 Boundary conditions for global domain 𝑥-max EQ.0: Free EQ.1: Rigid reflecting boundary IBCY0 Boundary conditions for global domain 𝑦-min EQ.0: Free EQ.1: Rigid reflecting boundary IBCY1 Boundary conditions for global domain 𝑦-max EQ.0: Free EQ.1: Rigid reflecting boundary VARIABLE DESCRIPTION IBCZ0 Boundary conditions for global domain 𝑧-min EQ.0: Free EQ.1: Rigid reflecting boundary IBCZ1 Boundary conditions for global domain 𝑧-max EQ.0: Free EQ.1: Rigid reflecting boundary BC_P Pressure ambient boundary condition for global domain EQ.0: Off (Default) EQ.1: On (Remark 2) Remarks: 1. Common Material Constants for commonly used High Explosives. IHETYPE 𝜌 TNT 1630 C4 1601 kg m3 kg m3 𝑒0 GJ m3 GJ m3 𝛾 COV D 1.35 0.6 6930 1.32 0.6 8193 2. Pressure Boundary Conditions. If pressure boundary conditions are used, particles will not escape from the global domain when the pressure in the do- main is lower than the ambient. The keyword *PERTURBATION provides a means of defining deviations from the designed structure such as buckling imperfections. These perturbations can be viewed in LS-PREPOST as user-defined fringe plots. Available options are: *PERTURBATION_MAT *PERTURBATION_NODE *PERTURBATION_SHELL_THICKNESS *PERTURBATION_OPTION Available options are: MAT NODE SHELL_THICKNESS Purpose: Define a perturbation (stochastic field) over the whole model or a portion of the model, typically to trigger an instability. The NODE option modifies the three dimensional coordinates for the whole model or a node set. For the SHELL_THICK- NESS option the shell thicknesses are perturbed for the whole model or a shell set. The MAT option perturbs a material parameter value for all the elements associated with that material. Material Perturbation Card. Card 1 for MAT keyword option. Perturb a material parameter. Card 1 1 2 3 4 5 6 7 8 Variable TYPE PID SCL CMP ICOORD CID Type Default I 1 I 0 F 1.0 I 7 I 0 I 0 Node Perturbation Card. Card 1 for NODE keyword option. Perturb the coordinates of a node set (or all nodes). Card 1 1 2 3 4 5 6 7 8 Variable TYPE NSID SCL CMP ICOORD CID Type Default I 1 I 0 F 1.0 I 7 I 0 I Shell Thickness Card. Card 1 for SHELL_THICKNESS keyword option. Perturb the thickness of a set of shells (or all shells). Card 1 1 2 3 4 5 6 7 8 Variable TYPE EID SCL ICOORD CID Type Default I 1 I 0 F 1.0 I 0 I 0 Harmonic Perturbation Cards (TYPE = 1). Card format 2 for TYPE = 1. Include as many cards of the following card as necessary. The input ends at the next keyword (“*”) card. Card 2 1 2 3 4 5 6 7 8 Variable AMPL XWL XOFF YWL YOFF ZWL ZOFF Type F F F F F F F Default 1.0 0.0 0.0 0.0 0.0 0.0 0.0 Fade Field Perturbation Card (TYPE = 2). Card format 2 for TYPE = 2. Card 2 1 2 3 4 5 6 7 8 Variable FADE Type F Default 1.0 Perturbation From File Card (TYPE = 3). Card format 2 for TYPE = 3. Card 2 1 2 3 4 5 6 7 8 Variable FNAME Type A Default none Spectral Field Perturbation Card (TYPE = 4). Card format 2 for TYPE = 4 (fade fiel).. Card 2 1 2 3 4 5 6 7 8 Variable CSTYPE ELLIP1 ELLIP2 RND Type I F F Default none 1.0 1.0 I 0 Spectral Perturbation Parameter Cards. Include One, two, or three cards of this format, depending on the value of CSTYPE. Card 3 1 2 3 4 5 6 7 8 Variable CFTYPE CFC1 CFC2 CFC3 Type I F F F Default none 1.0 1.0 1.0 VARIABLE DESCRIPTION TYPE Type of perturbation EQ.1: Harmonic Field EQ.2: Fade out all perturbations at this node set EQ.3: Read perturbations from a file EQ.4: Spectral field VARIABLE DESCRIPTION PID NSID EID SCL CMP Part ID. Node set ID. Specify 0 to perturb all the nodes in the model. Element set ID. Specify 0 to perturb all the elements in the model. Scale factor Component. For the NODE option, these are given below. For the MAT option, see the description of the material. EQ.1: 𝑥 coordinate EQ.2: 𝑦 coordinate EQ.3: 𝑧 coordinate EQ.4: 𝑥 and 𝑦 coordinate EQ.5: 𝑦 and 𝑧 coordinate EQ.6: 𝑧 and 𝑥 coordinate EQ.7: 𝑥, 𝑦, and 𝑧 coordinate ICOORD Coordinate system to use; see Remarks 7, 8 and 9 EQ.0: Global Cartesian EQ.1: Cartesian EQ.2: Cylindrical (computed and applied) EQ.3: Spherical (computed and applied) EQ.-2: Computed in cartesian but applied in cylindrical EQ.-3: Computed in cartesian but applied in spherical CID Coordinate system ID, see *DEFINE_COORDINATE_NODES AMPL Amplitude of the harmonic perturbation XWL XOFF YWL YOFF 𝑥 wavelength of the harmonic field 𝑥 offset of harmonic field 𝑦 wavelength of the harmonic field 𝑦 offset of harmonic field VARIABLE DESCRIPTION ZWL ZOFF FADE 𝑧 wavelength of the harmonic field 𝑧 offset of harmonic field Parameter controlling the distance over which all *PERTURBA- TION_NODE are faded to zero FNAME Name of file containing the perturbation definitions CSTYPE Correlation structure: EQ.1: 3D isotropic. The 𝑥, 𝑦 and 𝑧 correlations are described using one correlation function. Define CFC1. EQ.2: 3D product. The 𝑥, 𝑦 and 𝑧 correlations are described using a correlation function each. Define CFC1, CFC2 and CFC3. EQ.3: 2D isotropic. A correlation function describes the 𝑥 correlation while the 𝑦𝑧 isotropic relationship is de- scribed using another correlation function. Define CFC1 and CFC2. EQ.4: 2D isotropic. The 𝑥𝑧 isotropic relationship is described using a correlation function, while another correlation function describes the 𝑦 correlation while. Define CFC1 and CFC2. EQ.5: 2D isotropic. The 𝑥𝑦 isotropic relationship is described using a correlation function, while another correlation function describes the 𝑧 correlation while. Define CFC1 and CFC2. EQ.6: 3D elliptic. Define CSE1, CSE2 and CFC1. EQ.7: 2D elliptic. A correlation function describes the 𝑥 correlation while the 𝑦𝑧 elliptic relationship is described using another correlation function. Define CSE1 and CFC1. EQ.8: 2D elliptic. A correlation function describes the 𝑦 correlation while the 𝑧𝑥 elliptic relationship is described using another correlation function. Define CSE1 and CFC1. EQ.9: 2D elliptic. The 𝑥𝑦 elliptic relationship is described using a correlation function, while another correlation function describes the 𝑧 correlation while. Define CSE1 and VARIABLE DESCRIPTION CFC1. ELLIP1 Elliptic constant for 2D and 3D elliptic fields ELLIP2 Elliptic constant for 3D elliptic field RND Seed for random number generator. EQ.0: LS-DYNA will generate a random seed GT.0: Value to be used as seed CFTYPE Correlation function EQ.1: Gaussian EQ.2: Exponential EQ.3: Exponential Cosine EQ.4: Rational EQ.5: Linear CFCi Correlation function constant i Remarks: 1. Postprocessing. The perturbation can be viewed in LS-PrePost. For the NODE option, LS-DYNA creates files named pert_node_x/y/z/res, which can be viewed as user-defined fringe plots. For the SHELL_THICKNESS and MAT options, the files are named pert_shell_thickness and pert_mat respectively. If a coordinate system with a radial component is used, then the file pert_node_radial is also written. 2. Linear Combinations and Maximum Amplitudes. Perturbations specified using separate *PERTURBATION cards are created separately and then added together. This is true as well for special cases such as CMP = 7 in which case the 𝑥, 𝑦 and 𝑧 fields are created separately and added together afterwards, which can result in an absolute amplitude greater than specified using AMPL or SCL. 3. Harmonic Perturbations. The harmonic perturbation is 𝑝CMP(𝑥, 𝑦, 𝑧) = SCL × AMPL× [sin (2𝜋 𝑥 + XOFF XWL ) + sin (2𝜋 𝑦 + YOFF YWL ) + sin (2𝜋 𝑧 + ZOFF ZWL )] Note that the harmonic perturbations can sum to values greater than SCL × AMPL. 4. The Fade Perturbation. The fade perturbation is 𝑝′(𝑥, 𝑦, 𝑧) = 𝑆𝐶𝐿 × (1 − 𝑒FADE×𝑥′) 𝑝(𝑥, 𝑦, 𝑧) where 𝑥′ the shortest distance to a node in the node set specified and FADE the parameter controlling the sharpness of the fade perturbation. 5. Keyword Format for FNAME Field. The file FNAME must contain the perturbation in the LS-DYNA keyword format. This file can be created from the d3plot results using the LS-PrePost Output capability. The data must be arranged into two columns with the first column being the node ids. Lines starting with the character $ will be ignored. 6. Correlation Functions. The correlation functions are defined as follows: a) Gaussian: 𝐵(𝑡) = 𝑒−(𝑎𝑡)2 b) Exponential: 𝐵(𝑡) = 𝑒−|𝑎𝑡|𝑏 c) Exponent and Cosine: 𝐵(𝑡) = 𝑒−|𝑎𝑡|cos(𝑏𝑡) d) Rational: 𝐵(𝑡) = (1 + |𝑎𝑡|𝑏)−𝑐 e) Piecewise Linear: 𝐵(𝑡) = (1 − |𝑎𝑡|)𝜒(1 − |𝑎𝑡|) f) With 𝜒 the Heaviside step function and a, b and c corresponding to CFC1, CFC2 and CFC3. 7. Cylindrical Coordinates. For the cylindrical coordinate system option (ICOORD = 2), the default is to use the global coordinate system for the location of the cylindrical part, with the base of the cylinder located at the origin, and the global 𝑧-axis aligned with the cylinder axis. For cylindrical parts not located at the global origin, define a coordinate system (numbered CID) using *DE- FINE_COORDINATE_NODES by selecting any three nodes on the base of the cylinder in a clockwise direction (resulting in the local 𝑧-axis to be aligned with the cylinder). 8. Spherical Coordinates. For the spherical coordinate system (ICOORD = 3), the coordinates are the radius, zenith angle [0, 𝜋], and the azimuth an- gle [0,2𝜋]. The default is to use the global coordinate system with the zenith measured from the 𝑧-axis and the azimuth measured from the 𝑥-axis in the 𝑥𝑦- plane. For spherical parts not located at the global origin, define a coordinate system using *DEFINE_COORDINATE_NODES by selecting any three nodes as follows: the first node is the center of the sphere, the second specifies the 𝑥- axis of the coordinate system, while the third point specifies the plane contain- ing the new 𝑦-axis. The 𝑧-axis will be normal to this plane. 9. Computed In Cartesian Applied to Cylindrical or Spherical. It is possible to compute the perturbations in a Cartesian coordinate system, but to apply them in a cylindrical or spherical coordinate system (ICOORD = -2, -3). This is the natural method of doing say a radial perturbation of a sphere using a spectral perturbation field. We expect that computing the perturbation in the spherical coordinate system should be rare (ICOORD = 3). Computing a perturbation in a cylindrical coordinate system should be common though; for example, a cir- cumferential harmonic perturbation. 10. Material Perturbation Feature. Only *MAT_238 (*MAT_PERT_PIECEWISE_- LINEAR_PLASTICITY) and solid elements in an explicit analysis can be per- turbed using *PERTURBATION_MAT. See the documentation of this material for allowable components. Only one part per model can be perturbed. For some perturbed quantity c, the material perturbation is applied on an element- by-element basis as 𝑐new = (1 + 𝑝)𝑐base where 𝑝 is a random number, which is written to the pert_mat file during the calculation. Values of 𝑝 less than -1 are not allowed because the material behav- ior is not defined. Completely independent of *PERTURBATION_MAT, see *DEFINE_STOCHAS- TIC_VARIATION for a way to define a stochastic variation of yield stress and/or failure strain in material models 10, 15, 24, 81, and 98 and the shell version of material 123. . Two keywords are defined in this section. *RAIL_TRACK *RAIL_TRAIN *RAIL_TRACK Purpose: Wheel-rail contact algorithm intended for railway applications but can also be used for other purposes. The wheel nodes (defined on *RAIL_TRAIN) represent the contact patch between wheel and rail. A penalty method is used to constrain the wheel nodes to slide along the track. A track consists of two rails, each of which is defined by a set of beam elements. Card Sets. For each track include one pair of cards 1 and 2. This input ends at the next keyword (“*”) card. Card 1 Variable 1 ID 2 3 4 5 6 7 8 BSETID1 NORGN1 LCUR1 OSET1 SF1 GA1 IDIR Type I I I I F F F Default none none none none 0.0 1.0 0.0 Card 2 1 2 3 4 5 6 7 Variable blank BSETID2 NORGN2 LCUR2 OSET2 SF2 GA2 Type Default - - I I I F F F none none none 0.0 1.0 0.0 I 0 8 VARIABLE DESCRIPTION ID Track ID BSETID1,2 Beam set ID for rails 1 and 2 containing all beam elements that make up the rail, see *SET_BEAM. NORGN1,2 Reference node at one end of each rail, used as the origin for the roughness curve. The train will move in a direction away from this node. LCUR1,2 *RAIL DESCRIPTION Load curve ID defining track roughness (vertical displacement from line of beam elements) of the rail as a function of distance from the reference node NORIGIN. Distance from reference node on x-axis of curve, roughness on y-axis. Default: no roughness. OSET1,2 Origin of curve LCUR is shifted by distance OSET towards the reference node. SF1,2 GA1,2 IDIR Roughness values are scaled by SF. Default: 1.0. Shear stiffness of rail per unit length (used to calculate local rail GA = shear shear deformation within each beam element). modulus x cross-sectional area. Default: local shear deformation is ignored. Determines which way is “up” for purposes of wheel/rail contact. Vertical contact works like a normal penalty-based contact while horizontal contact follows Figure 34-2. EQ.0: (Default) global z is “up” and the global x-y plane is assumed horizontal irrespective of the geometry of the rails. EQ.1: “Up” is the normal vector to the plane containing the 2 rails, given by the vector c where c = (a x b), a is the direc- tion along rail 1 heading away from node NORGN1 and b is the vector from rail 1 to rail 2. Both a and b are de- termined locally at the contact point EQ.-1: Same as IDIR = 1 except “up” is along -c. Remarks: *RAIL_TRACK and *RAIL_TRAIN were written by Arup to represent wheel-rail contact. They have been used to generate loading on models of bridges for vibration predictions, stress calculations and for estimating accelerations experienced by passengers. Other non-railway uses are possible: the algorithm causes the “train” nodes to follow the line defined by the “rail” beam elements and transfers forces between them. In some cases (especially vibration modeling), double precision versions of LS-DYNA may give superior results because of the small relative deflections between wheel and rail. Theoretical curve Rail Node Beam element Roughness + = Distance Theoretical curve Surface profile = theoretical curve + roughness D= Distance of train node below surface profile Train node Force = VERTSTF × D Figure 34-1. Track Model Track modeling: The rails of the track should be modeled by two parallel lines of beam elements. The track can be curved or straight and the rails can be modeled as deformable or rigid. If required, rail pads, sleepers and ballast may also be modeled – typically with spring, damper and beam elements. It is also possible to use this algorithm to control the motion of simple road vehicle models: beam element “rails” made of null material can be embedded in the road surface. It is recommended that the mesh size of the two rails should be similar: LS-DYNA calculates a local coordinate system for each train node based on the alignment of the currently contacted beam element and the nearest node on the other rail. Because wheel-rail contact stiffness is generally very high, and wheel masses are large, small deviations from a straight line or smooth curve can lead to large transient forces. It is recommended that great care be taken in generating and checking the geometry for the track, especially where the track is curved. Some pre-processors write the coordinates with insufficient precision to the LS-DYNA input file, and this can cause unintended roughness in the geometry. For the same reason, if the line of the track were taken as straight between nodes, spurious forces would be generated when the wheel passes from one rail element to the next. This is avoided because the *RAIL algorithm calculates a theoretical curved centerline for the rail element to achieve continuity of slope from one element to the next. Where the length of the rail elements is similar to or shorter than the maximum section dimension, shear deformation may be significant and it is possible to include this in the theoretical centerline calculation to further reduce spurious forces at the element boundaries (inputs GA1, GA2). Roughness (small deviations in the vertical profile from a perfect straight line) does exist in real life and is a principal source of vibration. *RAIL allows the roughness to be modeled by a load curve giving the vertical deviation (in length units) of the rail surface from the theoretical centerline of the beam elements as a function of distance along the track from the origin node of the rail. The roughness curve is optional. Ideally, roughness profiles measured from both rails of the same piece of track should be used so that the relationship between bump and roll modes is correctly captured. Whether roughness is included or not, it is important to select as the origin nodes (NORIGIN1 and NORIGIN2) the nodes at the end of the rails away from which the train will be traveling. The train can start at any point along the rails but must travel away from the origin nodes. Train modeling: The vehicle models are typically modeled using spring, damper and rigid elements, or simply a point mass at each wheel position. Each node in the set referred to on *RAIL_- TRAIN represents the contact patch of one wheel (note: not the center of the wheel). These nodes should be initially on or near the line defined by either of the two rails. LS- DYNA will move the train nodes initially onto the rails to achieve the correct initial wheel-rail forces. If the results are viewed with magnified displacements, the initial movements can appear surprising. Wheel roughness input is available. This will be applied in addition to track roughness. The input curve must continue for the total rolled distance – it is not assumed to repeat with each wheel rotation. This is to avoid problems associated with ensuring continuity between the start and end of the profile around the wheel circumference, especially since the profiles might be generated from roughness spectra rather than taken directly from measured data. Lateral Force Force on Wheel B L3 L2 Deflection L2 L3 Force on Wheel A L2 L2 Figure 34-2. Illustration of lateral drift parameters L2 and L3 from *RAIL_- TRACK. Wheel-rail interface: The wheel-rail interface model is a simple penalty function designed to ensure that the train nodes follow the line of the track. It does not attempt to account for the shape of the rail profile. Vertical and lateral loads are treated independently. For this reason, the algorithm is not suitable for rail vehicle dynamics calculations. Wheel-rail contact stiffness is input on *RAIL_TRAIN. For vertical loads, a linear force- deflection relationship is assumed in compression; no tensile force is generated (this corresponds to the train losing contact with the rail). Typical contact stiffness is 2MN/mm. Lateral deflections away from the theoretical centerline of the rail beams are also penalized by a linear force-deflection relationship. The lateral force is applied only to wheels on the side towards which the train has displaced (corresponding to wheel flanges that run inside the rails). Optionally, a “gap” can be defined in input parameter L2 such that the wheel set can drift laterally by L2 length units before any lateral force is generated. A further option is to allow smooth transition between “gap” and “contact” by means of a transition distance input as parameter L3. Figure 34-2 illustrates the geometry of parameters L2 and L3. Generally, with straight tracks a simple linear stiffness is sufficient. With curved tracks, a reasonable gap and transition distance should be defined to avoid unrealistic forces being generated in response to small inaccuracies in the distance between the rails. Gravity loading is expected, in order to maintain contact between rail and wheel. This is normally applied by an initial phase of dynamic relaxation. To help achieve convergence quickly, or in some cases avoid the need for dynamic relaxation altogether, the initial force expected on each train node can be input (parameter FINIT on *RAIL_- TRAIN). LS-DYNA positions the nodes initially such that the vertical contact force will be FINIT at each node. If the suspension of the rail vehicles is modeled, it is recommended that the input includes carefully calculated precompression of the spring elements; if this is not done, achieving initial equilibrium under gravity loading can be very time consuming. The *RAIL algorithm ensures that the train follows the rails, but does not provide forward motion. This is generally applied using *INITIAL_VELOCITY, or for straight tracks, *BOUNDARY_PRESCRIBED_MOTION. Output: LS-DYNA generates an additional ASCII output file train_force_n, where n is an integer updated to avoid overwriting any existing files. The file contains the forces on each train node, output at the same time intervals as the binary time history file (DT on *DATABASE_BINARY_D3THDT). Checking: It is recommended that track and train models be tested separately before adding the *RAIL cards. Check that the models respond stably to impulse forces and that they achieve equilibrium under gravity loading. The majority of problems we have encountered have been due to unstable behavior of train or track. Often, these are first detected by the *RAIL algorithm and an error message will result. *RAIL_TRAIN Purpose: Define train properties. A train is defined by a set of nodes in contact with a rail defined by *RAIL_TRACK. Card Sets. For each train include one pair of cards 1 and 2. This input ends at the next keyword (“*”) card. Card 1 Variable 1 ID 2 3 4 5 6 7 8 NSETID (omit) FINIT (omit) TRID LCUR OFFS Type I I F F F Default none none 0.0 0.0 0.0 Card 2 1 2 Variable VERTSTF LATSTF Type F F 3 V2 F 4 V3 F 5 L2 F I F none 0.0 7 8 I 0 6 L3 F Default 0.0 0.0 0.0 0.0 0.0 0.0 VARIABLE DESCRIPTION ID Train ID NSETID Node set ID containing all nodes that are in contact with rails. (omit) FINIT (omit) TRID Unused variable – leave blank. Estimate of initial vertical force on each wheel (optional) – speeds up the process of initial settling down under gravity loading. Unused variable – leave blank. ID of track for this train, see *RAIL_TRACK. LCUR *RAIL DESCRIPTION ID Load curve containing wheel roughness (distance of wheel surface away from perfect circle) vs. distance traveled. The curve does not repeat with each rotation of the wheel – the last point should be at a greater distance than the train is expected to travel. Default: no wheel roughness. OFFS Offset distance used to generate different roughness curves for each wheel from the roughness curve LCUR. The curve is offset on the x-axis by a different whole number multiple of OFFS for each wheel. VERTSTF Vertical stiffness of rail contact. LATSTF Lateral stiffness of rail contact. V2,V3 Unused variables – leave blank. L2 L3 Lateral clearance from rail to wheel rim. Lateral force is applied to a wheel only when it has moved more than L2 away from the other rail, i.e. the wheel rims are assumed to be near the inner face of the rail. Further lateral distance before full lateral stiffness applies (force- deflection curve follows a parabola up to this point). Two keywords are used in this section to define rigid surfaces: *RIGIDWALL_GEOMETRIC_OPTION_{OPTION}_{OPTION}}_{OPTION} *RIGIDWALL_PLANAR_{OPTION}_{OPTION}_{OPTION} The RIGIDWALL option provides a simple way of treating contact between a rigid surface and nodal points of a deformable body, called slave nodes. Slave nodes which belong to rigid parts are not, in general, checked for contact with only one exception. The RIGIDWALL_PLANAR option may be used with nodal points of rigid bodies if the planar wall defined by this option is fixed in space and the RWPNAL parameter is set to a positive nonzero value on the control card, *CONTROL_CONTACT. When the rigid wall defined in this section moves with a prescribed motion, the equations of rigid body mechanics are not involved. For a general rigid body treatment with arbitrary surfaces and motion, refer to the *CONTACT_ENTITY definition. The *CONTACT_ENTITY option is for treating contact between rigid and deformable surfaces only. Energy dissipated due to rigidwalls (sometimes called stonewall energy or rigidwall energy) is computed only if the parameter RWEN is set to 2 in *CONTROL_ENERGY. *RIGIDWALL_FORCE_TRANSDUCER Purpose: Define a force transducer for a rigid wall. The output of the transducer is written to the rwforc file. Card 1 1 2 3 4 5 6 7 8 Variable TID RWID Type I I Default none none . VARIABLE DESCRIPTION TID Transducer ID. RWID Rigid wall ID. Card 2 1 2 3 4 5 6 7 8 Variable Type Default Remarks HEADING C none Node Set Cards. For each node set add one card. This input ends at the next keyword (“*”). Card 3 1 2 3 4 5 6 7 8 Variable NSID Type I Default 0. . Remarks VARIABLE DESCRIPTION NSID Node set ID. Remarks: 1. The forces acting on rigid wall RWID are reported separately for each NSID. 2. For rigid walls using the segment option, the forces acting on each segment are reported separately for each NSID. *RIGIDWALL_GEOMETRIC_OPTION_{OPTION}_{OPTION}_{OPTION} Available options include: FLAT PRISM CYLINDER SPHERE If prescribed motion is desired an additional option is available: MOTION One of the shape types [FLAT, PRISM, CYLINDER, SPHERE] must be specified, followed by the optional definition of MOTION, both on the same line with *RIGID- WALL_GEOMETRIC. If an ID number is specified the additional option is available: ID If active, the ID card is the first card following the keyword. To view the rigid wall, the option: DISPLAY is available. With this option a rigid body is automatically defined which represents the shape, the physical position of the wall, and follows the walls motion if the MOTION option is active. Additional input is optional if DISPLAY is active. For the CYLINDER and SPHERE, the option: INTERIOR is available. Nodes are confined to the interior of these geometric forms. Purpose: Define a rigid wall with an analytically described form. Four forms are possible. A prescribed motion is optional. For general rigid bodies with arbitrary surfaces and motion, refer to the *CONTACT_ENTITY definition. This option is for treating contact between rigid and deformable surfaces only. Card Sets. For each rigid wall matching the specified keyword options include one set of the following data cards. This input ends at the next keyword (“*”) card. ID Card. Additional card for ID keyword option. Card 1 1 2 3 4 5 6 7 8 Variable RWID Type I HEADING A70 This heading is picked up by some of the peripheral LS-DYNA codes to aid in post- processing. VARIABLE DESCRIPTION RWID Rigid wall ID. This must be a unique number. HEADING Rigid wall descriptor. It is suggested that unique descriptions be used. Card 2 1 2 3 4 5 6 7 8 Variable NSID NSIDEX BOXID BIRTH DEATH Type I Default none I 0 I 0 F F 0. 1.0E+20 VARIABLE DESCRIPTION NSID Nodal set ID containing slave nodes, see *SET_NODE_OPTION: EQ.0: all nodes are slave to rigid wall. NSIDEX BOXID BIRTH Nodal set ID containing nodes that exempted as slave nodes, see *SET_NODE_OPTION. If defined, only nodes in box are included as slave nodes to rigid wall. Birth time of rigid wall. The time values of the load curves that control the motion of the wall are offset by the birth time. DESCRIPTION Death time of rigid wall. At this time the wall is deleted from the calculation. If dynamic relaxation is active at the beginning of the calculation and if BIRTH = 0.0, the death time is ignored during the dynamic relaxation. 2 YT F 0. 3 ZT F 0. 4 XH F 0. 5 YH F 0. 6 ZH F 0. 7 8 FRIC F 0. VARIABLE DEATH Card 3 Variable 1 XT Type F Default 0. Remarks VARIABLE DESCRIPTION XT YT ZT XH YH ZH 𝑥-coordinate of tail of any outward drawn normal vector, 𝐧, originating on wall (tail) and terminating in space (head), see Figure 35-1. 𝑦-coordinate of tail of normal vector 𝐧 𝑧-coordinate of tail of normal vector 𝐧 𝑥-coordinate of head of normal vector 𝐧 𝑦-coordinate of head of normal vector 𝐧 𝑧-coordinate of head of normal vector 𝐧 FRIC Coulomb friction coefficient except as noted below. EQ.0.0: frictionless sliding after contact, EQ.1.0: stick condition after contact. rectangular prism cylinder flat surface sphere Figure 35-1. Vector 𝐧 determines the orientation of the rigidwall. By including the MOTION option, motion of the rigidwall can be prescribed in any direction 𝐕 as defined by variables VX, VY, VZ. Flat Rigidwall Card. Card 4 for FLAT keyword option. A plane with a finite size or with an infinite size can be defined, see Figure 35-1. The vector m is computed as the vector cross product 𝐧 × 𝐥. The origin, which is the tail (the start) of the normal vector, is the corner point of the finite size plane. Card 4 1 2 3 4 5 6 7 8 Variable XHEV YHEV ZHEV LENL LENM Type F Default 0. F 0. F F F 0. infinity infinity VARIABLE DESCRIPTION XHEV YHEV ZHEV LENL 𝑥-coordinate of head of edge vector 𝐥, see Figure 35-1. 𝑦-coordinate of head of edge vector 𝐥 𝑧-coordinate of head of edge vector 𝐥 Length of 𝐥 edge. A zero value defines an infinite size plane. LENM Length of 𝐦 edge. A zero value defines an infinite size plane. Prismatic Rigidwall Card. Card 4 for PRISM keyword option. The description of the definition of a plane with finite size is enhanced by an additional length in the direction negative to 𝐧, see Figure 35-1. Card 4 1 2 3 4 5 6 7 8 Variable XHEV YHEV ZHEV LENL LENM LENP Type F F F F F F Default none 0. 0. infinity infinity infinity VARIABLE DESCRIPTION XHEV YHEV ZHEV LENL LENM LENP 𝑥-coordinate of head of edge vector 𝐥, see Figure 35-1. 𝑦-coordinate of head of edge vector 𝐥 𝑧-coordinate of head of edge vector 𝐥 Length of 𝐥 edge. A zero value defines an infinite size plane. Length of 𝐦 edge. A zero value defines an infinite size plane. Length of prism in the direction negative to 𝐧, see Figure 35-1. Cylinderical Rigidwall Card. Card 4 for CYLINDER keyword option. The tail of 𝐧 specifies the top plane of the cylinder. The length is defined in the direction negative to 𝐧. See Figure 35-1. Card 4 1 2 3 4 5 6 7 8 Variable RADCYL LENCYL NSEGS Type F F I Default none infinity none VARIABLE DESCRIPTION RADCYL Radius of cylinder LENCYL Length of cylinder, see Figure 35-1. Only if a value larger than zero is specified is a finite length assumed. NSEGS Number of subsections NSEGS Card. Additional card for NSEGS option. Card 5 Variable 1 VL 2 3 4 5 6 7 8 HEIGHT Type F F Default none none VARIABLE DESCRIPTION VL Distance from the Cylinder base HEIGHT Section height Spherical Rigidwall Card. Card 4 for SPHERE keyword option. The center of the sphere is identical to the tail (start) of 𝐧, see Figure 35-1. Card 4 1 2 3 4 5 6 7 8 Variable RADSPH Type F Default 0. VARIABLE DESCRIPTION RADSPH Radius of sphere Motion Card. Additional card for motion keyword option. Card 5 1 2 Variable LCID OPT Type I I 3 VX F 4 VY F 5 VZ F Default none none none none none VARIABLE DESCRIPTION 6 7 8 LCID OPT VX VY VZ Rigidwall motion curve number, see *DEFINE_CURVE. Type of motion: EQ.0: velocity specified, EQ.1: displacement specified. 𝑥-direction cosine of velocity/displacement vector 𝑦-direction cosine of velocity/displacement vector 𝑧-direction cosine of velocity/displacement vector Display Card. Optional card for DISPLAY keyword option. If this card is omitted default values are set. The values set here have no effect on the solution other than the PID appearing in the postprocessing. 5 6 7 8 Card 6 1 Variable PID Type I 2 RO I 3 E I 4 PR F Default none 1.0E-09 1.0E-04 0.3 VARIABLE DESCRIPTION PID RO E PR Unique part ID for moving geometric rigid wall. If zero, a part ID will be set that is larger than the maximum of all user defined part ID’s. Density of rigid wall. The default is set to 1.0E-09. Young’s modulus. The default is set to 1.0E-04. Poisson’s ratio. The default is set to 0.30. $$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ $ $$$$ *RIGIDWALL_GEOMETRIC_SPHERE_MOTION $ $$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ $ $ Define a rigid sphere: $ - with a radius of 8 $ - centered at (x,y,z) = (20,20,9) $ - that moves in the negative z-direction with a specified displacement $ given by a load curve (load curve: lcid = 5) $ - which prevents all nodes within a specified box from penetrating the $ sphere (box number: boxid = 3), these nodes can slide on the sphere $ without friction $ *RIGIDWALL_GEOMETRIC_SPHERE_MOTION $...>....1....>....2....>....3....>....4....>....5....>....6....>....7....>....8 $ nsid nsidex boxid 3 $ $ xt yt zt xh yh zh fric 20.0 20.0 9.0 20.0 20.0 0.0 0.0 $ $ radsph 8.0 $ $ lcid opt vx vy vz 5 1 0.0 0.0 -1.0 $ $ *DEFINE_BOX $ boxid xmn xmx ymn ymx zmn zmx 3 0.0 40.0 0.0 40.0 -1.0 1.0 $ $ *DEFINE_CURVE $ lcid sidr scla sclo offa offo 5 $ abscissa ordinate 0.0 0.0 0.0005 15.0 $ $$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ *RIGIDWALL_PLANAR_{OPTION}_{OPTION}_{OPTION} Available options include: <BLANK> ORTHO FINITE MOVING FORCES The ordering of the options in the input below must be observed but the ordering of the options on the command line is unimportant, i.e.; the ORTHO card is first, the FINITE definition card below must precede the MOVING definition card, and the FORCES definition card should be last. The ORTHO option does not apply if the MOVING option is used. An ID number may be assigned to the rigid wall using the following option: ID If this option is active, the ID card is the first card following the keyword. Display of a non-moving, planar rigid wall is on by default . The option DISPLAY is available for display of moving rigid walls. With this option active, a rigid body is automatically created which represents the shape of the rigid wall and tracks its position without need for additional input. The part ID of the rigid body defaults to RWID if the ID option is active, and if RWID is a unique ID within the set of all part IDs. Purpose: Define planar rigid walls with either finite (FINITE) or infinite size. Orthotropic friction can be defined (ORTHO). Also, the plane can possess a mass and an initial velocity (MOVING); otherwise, the wall is assumed to be stationary. The FORCES option allows the specification of segments on the rigid walls on which the contact forces are computed. In order to achieve a more physical reaction related to the force versus time curve, the SOFT value on the FORCES card can be specified. Card Sets. For each rigid wall matching the specified keyword options include one set of the following data cards. This input ends at the next keyword (“*”) card. ID. Card. Additional card for ID keyword option. Card 1 1 2 3 4 5 6 7 8 Variable RWID Type I Default none VARIABLE DESCRIPTION RWID Rigid wall ID. Up to 8 characters can be used. Card 2 1 2 3 4 5 6 7 8 Variable NSID NSIDEX BOXID OFFSET BIRTH DEATH RWKSF Type I Default none I 0 I 0 F 0. F F F 0. 1.0E+20 1.0 VARIABLE DESCRIPTION NSID Nodal set ID containing slave nodes, see *SET_NODE_OPTION: EQ.0: all nodes are slave to rigid wall. NSIDEX BOXID OFFSET Nodal set ID containing nodes that exempted as slave nodes, see *SET_NODE_OPTION. All nodes in box are included as slave nodes to rigid wall, see *DEFINE_BOX. If options NSID or NSIDEX are active then only the subset of nodes activated by these options are checked to see if they are within the box. All nodes within a normal offset distance, OFFSET, to the rigid wall are included as slave nodes for the rigid wall. If options NSID, NSIDEX, or BOXID are active then only the subset of nodes activated by these options are checked to see if they are within the offset distance. This option applies to the PLANAR wall only. *RIGIDWALL Tail of normal vector is the origin and corner point if extent of stonewall is finite. Figure 35-2. Vector 𝐧 is normal to the rigidwall. An optional vector 𝐥 can be defined such that 𝐦 = 𝐧 × 𝐥. The extent of the rigidwall is limited by defining L (LENL) and M (LENM). A zero value for either of these lengths indicates that the rigidwall is infinite in that direction. VARIABLE DESCRIPTION BIRTH DEATH RWKSF Birth time of rigid wall. The time values of the load curves that control the motion of the wall are offset by the birth time. Death time of rigid wall. At this time the wall is deleted from the calculation. If dynamic relaxation is active at the beginning of the calculation and if BIRTH = 0.0, the death time is ignored during the dynamic relaxation. Stiffness scaling factor. If RWKSF is also specified in *CON- TROL_CONTACT, the stiffness is scaled by the product of the two values. Card 3 Variable 1 XT Type F Default 0. 2 YT F 0. 3 ZT F 0. 4 XH F 0. 5 YH F 0. 6 ZH F 0. 7 8 FRIC WVEL F 0. F 0. VARIABLE DESCRIPTION XT YT ZT XH YH ZH 𝑥-coordinate of tail of any outward drawn normal vector, 𝐧, originating on wall (tail) and terminating in space (head), see Figure 35-2. 𝑦-coordinate of tail of normal vector 𝐧 𝑧-coordinate of tail of normal vector 𝐧 𝑥-coordinate of head of normal vector 𝐧 𝑦-coordinate of head of normal vector 𝐧 𝑧-coordinate of head of normal vector 𝐧 FRIC Coulomb friction coefficient except as noted below. EQ.0.0: frictionless sliding after contact, EQ.1.0: no sliding after contact, EQ.2.0: node is welded after contact with frictionless sliding. Welding occurs if and only if the normal value of the impact velocity exceeds the critical value specified by WVEL. EQ.3.0: node is welded after contact with no sliding. Welding occurs if and only if the normal value of the impact ve- locity exceeds the critical value specified by WVEL. In summary, FRIC could be any positive value. Three special values of FRIC trigger special treatments as follows: FRIC 1.0 2.0 3.0 Bouncing back from wall allowed not allowed not allowed Sliding on wall not allowed allowed not allowed WVEL Critical normal velocity at which nodes weld to wall (FRIC = 2 or 3). input Node 2 points from node 1 to 2 Node 1 defintion by nodes b = n × d a = b × n definition by vector components Figure 35-3. Definition of orthotropic friction vectors. The two methods of defining the vector, 𝐝, are shown. If vector 𝐝 is defined by nodes 1 and 2, the local coordinate system may rotate with the body which contains the nodes; otherwise, 𝐝 is fixed in space, thus on the rigid wall, and the local system is stationary. Orthotropic Friction Card 1. Additional card for ORTHO keyword option. See Figure 35-3 for the definition of orthotropic friction. Card 4 1 2 3 4 5 6 7 8 Variable SFRICA SFRICB DFRICA DFRICB DECAYA DECAYB Type F Default 0. F 0. F 0 F 0 F 0. F 0. Orthotropic Friction Card 2. Additional card for ORTHO keyword option. See Figure 35-3 for the definition of orthotropic friction. Card 5 1 2 Variable NODE1 NODE2 Type I Default 0. I 0. 3 D1 F 0 4 D2 F 0 5 D3 F 0. 6 7 8 VARIABLE DESCRIPTION SFRICA SFRICB LS-DYNA R10.0 Static friction coefficient in local a-direction, 𝜇𝑠𝑎, see Figure 35-3 VARIABLE DESCRIPTION DFRICA Dynamic friction coefficient in local 𝑎-direction, 𝜇𝑘𝑎 DFRICB Dynamic friction coefficient in local 𝑏-direction, 𝜇𝑘𝑏 DECAYA Decay constant in local 𝑎-direction, 𝑑𝑦𝑎 DECAYB Decay constant in local 𝑏-direction, 𝑑𝑦𝑏 NODE1 Node 1, alternative to definition with vector 𝐝 below. See Figure 35-3. With the node definition the direction changes if the nodal pair rotates. NODE2 Node 2 𝑑1, 𝑥-component of vector, alternative to definition with nodes above. See Figure 35-3. This vector is fixed as a function of time. 𝑑2, 𝑦-component of vector 𝑑3, 𝑧-component of vector D1 D2 D3 Remarks: 1. The coefficients of friction are defined in terms of the static, dynamic and decay coefficients and the relative velocities in the local a and b directions as 𝜇𝑎 = 𝜇𝑘𝑎 + (𝜇𝑠𝑎𝜇𝑘𝑎)𝑒𝑑𝑣𝑎𝑉relative,𝑎 𝜇𝑏 = 𝜇𝑘𝑏 + (𝜇𝑠𝑏𝜇𝑘𝑏)𝑒𝑑𝑣𝑏𝑉relative,𝑏 2. Orthotropic rigid walls can be used to model rolling objects on rigid walls where the frictional forces are substantially higher in a direction transverse to the rolling direction. To use this option define a vector 𝒅 to determine the local frictional directions via: 𝐛 = 𝐧 × 𝐝, 𝐚 = 𝐛 × 𝐧 where 𝐧 is the normal vector to the rigid wall. If 𝐝 is in the plane of the rigid wall, then 𝐚 is identical to 𝐝. Finite Wall Size Card. Additional card for FINITE keyword option. See Figure 35-3 for the definition of orthotropic friction. See Figure 35-2. The 𝒎 vector is computed as the vector cross product 𝒎 = 𝒏 × 𝒍. The origin, the tail of the normal vector, is taken as the corner point of the finite size plane. Card 6 1 2 3 4 5 6 7 8 Variable XHEV YHEV ZHEV LENL LENM Type F Default 0. F 0. F F F 0. infinity infinity VARIABLE DESCRIPTION XHEV YHEV ZHEV LENL x-coordinate of head of edge vector 𝒍, see Figure 35-2. y-coordinate of head of edge vector 𝒍 z-coordinate of head of edge vector 𝒍 Length of 𝒍 edge LENM Length of 𝒎 edge Moving Wall Card. Additional card for MOVING keyword option. Note: The MOVING option is not compatible with the ORTHO option. 3 4 5 6 7 8 Card 7 1 Variable MASS Type F 2 V0 F Default none 0. VARIABLE DESCRIPTION MASS Total mass of rigidwall V0 Initial velocity of rigidwall in direction of defining vector, n Forces Card. Additional card for FORCES keyword option. This option allows the force distribution to be monitored on the plane. Also four points can be defined for visualization of the rigid wall. A shell or membrane element must be defined with these four points as the connectivity for viewing in LS-PREPOST. 7 8 Card 7 1 2 Variable SOFT SSID Type Default I 0 Remarks I 0 1 3 N1 I 0 2 4 N2 I 0 5 N3 I 0 6 N4 I 0 VARIABLE DESCRIPTION SOFT SSID Number of cycles to zero relative velocity to reduce force spike Segment set identification number for defining areas for force output, see *SET_SEGMENT and remark 1 below. N1-N4 Optional node for visualization Remarks: 1. The segment set defines areas for computing resultant forces. These segments translate with the moving rigidwall and allow the forced distribution to be determined. The resultant forces are written in file “RWFORC.” 2. These four nodes are for visualizing the movement of the wall, i.e., they move with the wall. To view the wall in LS-PREPOST it is necessary to define a single shell element with these four nodes as its connectivity. The single element must be deformable (non rigid) or else the segment will be treated as a rigid body and the nodes will have their motion modified independently of the rigidwall. $$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ $ $$$$ *RIGIDWALL_PLANAR_MOVING_FORCES $ $$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ $ $ Define a moving planar rigid wall: $ - that is parallel to the y-z plane starting at x = 250 mm $ - with an initial velocity of 8.94 mm/ms in the negative z-direction $ - that has a mass of 800 kg $ - which prevents all nodes in the model from penetrating the wall $ - with a friction coefficient for nodes sliding along the wall of 0.1 $ - track the motion of the wall by creating a node (numbered 99999) $ at the tail of the wall and assigning the node to move with the wall $ *RIGIDWALL_PLANAR_MOVING_FORCES $...>....1....>....2....>....3....>....4....>....5....>....6....>....7....>....8 $ nsid nsidex boxid 0 0 0 $ $ xt yt zt xh yh zh fric 250.0 0.0 0.0 0.0 0.0 0.0 0.1 $ $ SW mass SW vel 800.00 8.94 $ $ soft ssid node1 node2 node3 node4 0 0 99999 $ $ *NODE $ $...>....1....>....2....>....3....>....4....>....5....>....6....>....7....>....8 $ nid x y z tc rc 99999 250.0 0.0 0.0 0 0 $ $ *DATABASE_HISTORY_NODE $ Define nodes that output into nodout $ id1 id2 id3 $...>....1....>....2....>....3....>....4....>....5....>....6....>....7....>....8 99999 $ *DATABASE_NODOUT $ dt 0.1 $ $$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ In this section, the element formulation, integration rule, nodal thicknesses, and cross sectional properties are defined. All section identifiers (SECID’s) defined in this section must be unique, i.e., if a number is used as a section ID for a beam element then this number cannot be used again as a section ID for a solid element. The keyword cards in this section are defined in alphabetical order: *SECTION_ALE1D *SECTION_ALE2D *SECTION_BEAM_{OPTION} *SECTION_BEAM_AISC *SECTION_DISCRETE *SECTION_POINT_SOURCE *SECTION_POINT_SOURCE_MIXTURE *SECTION_SEATBELT *SECTION_SHELL_{OPTION} *SECTION_SOLID_{OPTION} *SECTION_SPH_{OPTION} *SECTION_TSHELL The location and order of these cards in the input file are arbitrary. An additional option TITLE may be appended to all the *SECTION keywords. If this option is used then an addition line is read for each section in 80a format which can be used to describe the section. At present LS-DYNA does make use of the title. Inclusion of titles gives greater clarity to input decks. *SECTION_ALE1D Purpose: Define section properties for 1D ALE elements Card Sets. For each ALE1D section add one pair of cards 1 and 2. This input ends at the next keyword (“*”) card. Card 1 1 2 3 4 5 6 7 8 Variable SECID ALEFORM AET ELFORM I none 4 5 6 7 8 I 0 3 Type I/A I Default none none Card 2 1 2 Variable THICK THICK Type F F Default none none VARIABLE SECID DESCRIPTION Section ID. SECID is referenced on the *PART card. A unique number or label must be specified. ALEFORM ALE formulation: EQ.11: Multi-Material ALE formulation. AET Ambient Element Type EQ.4: Pressure inflow ELFORM Element formulation: EQ.7: Plane strain EQ.8: Axisymmetric (per radian) EQ.-8: spherical (per unit of solid angle) VARIABLE DESCRIPTION THICK Nodal thickness. See Remark 1 Remarks: 1. *SECTION_ALE1D is using the common *SECTION_BEAM reader which expects two thickness values. However, the ALE 1D will simply take the aver- age of these two values as the beam thickness. The thickness is not used for ELFORM = -8 but the reader routine expects val- ues on the 2nd line. *SECTION_ALE2D Purpose: Define section properties for 2D ALE elements. This supersedes the old way of defining section properties for 2D ALE elements via *SECTION_SHELL. For coupling between 2D Lagrangian elements and 2D ALE elements, use *CON- STRAINED_LAGRANGE_IN_SOLID rather than *CONTACT_2D_AUTOMATIC_SUR- FACE_IN_CONTINUUM. In the case of an axisymmetric analysis, ELFORM for *SECTION_ALE2D can only be set to 14 (area-weighted). In the same analysis, axisymmetric Lagrangian elements are not restricted to an area-weighted formulation. In other words, shell formulation 14 or 15 are permitted for Lagrangian shells and beam formulation 8 is permitted for Lagrangian beams. Coupling forces between the axisymmetric ALE elements and axisymmetric Lagrangian elements are automatically adjusted as needed. Section Cards. For each ALE2D section include a card. This input terminates at the next keyword (“*”) card. Card 1 1 2 3 4 5 6 7 8 Variable SECID ALEFORM AET ELFORM Type I/A I Default none none I 0 I none VARIABLE SECID DESCRIPTION Section ID. SECID is referenced on the *PART card. A unique number or label must be specified. ALEFORM ALE formulation: EQ.11: Multi-Material ALE formulation. VARIABLE DESCRIPTION AET Part type flag EQ.0: This is a regular or non-ambient part (default) EQ.4: Reservoir or ambient type part EQ.5: Reservoir or ambient type part, but only used together with *LOAD_BLAST_ENHANCED (LBE). It defines this part as an “ambient receptor part” for the transient blast load supplied by a corresponding LBE KW . ELFORM Element formulation: EQ.13: Plane strain (x-y plane) EQ.14: Axisymmetric solid (x-y plane, y-axis of symmetry) – area weighted *SECTION_BEAM_{OPTION} Available options include: <BLANK> AISC such that the keyword cards appear: *SECTION_BEAM *SECTION_BEAM_AISC Purpose: Define cross sectional properties for beam, truss, discrete beam, and cable elements. The AISC option may be used to specify standard steel sections as specified by the American Institute of Steel Construction, and is described separately after *SECTION_- BEAM Card Sets. For each BEAM section in the model add one set of the following 2 (maybe 3 for ELFORM = 12) cards. This input ends at the next keyword (“*”) card. Card 1 1 2 3 4 5 6 7 8 Variable SECID ELFORM SHRF QR/IRID CST SCOOR NSM Type I/A Default none I 1 F F F F F 1.0 2.0 0.0 0.0 0.0 Integrated Beam Card (types 1 and 11). Card 2 for ELFORM set to either type 1 or 11. Card 2 1 2 3 4 5 6 7 8 Variable TS1 TS2 TT1 TT2 NSLOC NTLOC Type F F F F F Resultant Beam With Shape Card (types 2, 3, and 12). Card 2 for ELFORM equal to 2, 3, or 12 and when first 7 characters of the card spell out “SECTION”. Card 2 1 2 3 4 5 6 7 8 Variable STYPE D1 D2 D3 D4 D5 D6 Type A10 F F F F F Resultant Beam Card 1 (types 2, 12, and 13). Card 2 for ELFORM equal to 2, 12, or 13 and when first 7 characters of card do not spell “SECTION”. Card 2 Variable Type 1 A F 2 3 ISS ITT F F 4 J F 5 6 7 8 SA IST F F Resultant Beam Card 2 (type 12 only). Card 3 for ELFORM equal to 12 and when first 7 characters of card 2 do not spell “SECTION”. Card 3 1 2 3 4 5 6 7 8 Variable YS ZS IYR IZR IRR IW IWR Type F F F F F F F Resultant Beam Card (type 3). Card 2 for ELFORM equal to 3. Card 2 Variable Type 1 A F 2 3 4 5 6 7 8 RAMPT STRESS F Integrated Beam Card (types 4 and 5). Card 2 for ELFORM equal to 4 or 5. Card 2 1 2 3 4 5 6 7 8 Variable TS1 TS2 TT1 TT2 Type F F F F Discrete Beam Card (type 6). Card 2 for ELFORM equal to 6 for any material other than material type 146. Card 2 1 2 3 4 5 6 7 8 Variable VOL INER CID CA OFFSET RRCON SRCON TRCON Type F F F F F F F F Discrete Beam Card (type 6, mat 146). Card 2 for ELFORM equal to 6 for material type 146. Card 2 1 2 3 4 5 6 7 8 Variable VOL INER CID DOFN1 DOFN2 Type F F F F F 2D Shell Card (types 7 and 8). Card 2 for ELFORM equal to 7 or 8. Card 2 1 2 3 4 5 6 7 8 Variable TS1 TS2 TT1 TT2 Type F F F Spot Weld Card (type 9). Card 2 for ELFORM equal to 9. Card 2 1 2 3 4 5 6 7 8 Variable TS1 TS2 TT1 TT2 PRINT Type F F F F F Integrated Beam Card (types 14). Card 2 for ELFORM equal to 14. Card 2 1 2 3 4 5 6 7 8 Variable PR IOVPR IPRSTR Type F F F F VARIABLE SECID DESCRIPTION Section ID. SECID is referenced on the *PART card. A unique number or label must be specified. ELFORM Element formulation options: EQ.1: Hughes-Liu with cross section integration (default), EQ.2: Belytschko-Schwer resultant beam (resultant), EQ.3: truss (resultant). See Remark 2. EQ.4: Belytschko-Schwer full cross-section integration, EQ.5: Belytschko-Schwer tubular beam with cross-section integration, EQ.6: discrete beam/cable, EQ.7: 2D plane strain shell element (𝑥𝑦 plane), EQ.8: 2D axisymmetric volume weighted shell element (𝑥𝑦 plane, 𝑦-axis of symmetry), EQ.9: spotweld beam, see *MAT_SPOTWELD. EQ.11: integrated warped beam. See Remark 4) EQ.12: resultant warped beam EQ.13: small displacement, linear Timoshenko beam with exact stiffness. See Remark 6 EQ.14: Elbow integrated tubular beam element. An user VARIABLE DESCRIPTION SHRF QR/IRID defined integration rule with tubular cross section (9) must be used. Note that the 2D and 3D element types must not be mixed, and different types of 2D elements must not be used together. For example, the plane strain element type must not be used with the axisymmetric element type. In 3D the different beam elements types, i.e., 1-6 and 9 can be freely mixed together. Shear factor. This factor is not needed for truss, resultant beam, discrete beam, and cable elements. The recommended value for rectangular sections is 5/6, the default is 1.0. Quadrature rule or rule number for user defined rule for integrated beams. See Remark 10 regarding beam formulations 7 and 8. EQ.1.0: one integration point, EQ.2.0: 2 × 2 Gauss quadrature (default beam), EQ.3.0: 3 × 3 Gauss quadrature, EQ.4.0: 3 × 3 Lobatto quadrature, EQ.5.0: 4 × 4 Gauss quadrature EQ.-n: where |n| is the number of the user defined rule. IRID integration rule n is defined using *INTEGRA- TION_BEAM card. CST Cross section type, not needed for truss, resultant beam, discrete beam, and cable elements: EQ.0.0: rectangular, EQ.1.0: tubular (circular only), EQ.2.0: arbitrary (user defined integration rule). SCOOR Affects the discrete beam formulation and also the update of the local coordinate system of the discrete beam element. This parameter does not apply to cable elements. The force and moment resultants in the output databases are output in the local coordinate system. See Remark 9 for more on the local coordinate system update. EQ.-13.0: Like -3.0, but with correction for beam rotation VARIABLE DESCRIPTION EQ.-12.0: Like -2.0, but with correction for beam rotation EQ.-3.0: beam node 1, the angular velocity of node 1 rotates triad, EQ.-2.0: beam node 1, the angular velocity of node 1 rotates triad but the r-axis is adjusted to lie along the line between the two beam nodal points. This option is not recommended for zero length discrete beams., EQ.-1.0: beam node 1, the angular velocity of node 1 rotates triad, EQ.0.0: centered between beam nodes 1 and 2, the average angular velocity of nodes 1 and 2 is used to rotate the triad, EQ.+1.0: beam node 2, the angular velocity of node 2 rotates triad. EQ.+2.0: beam node 2, the angular velocity of node 2 rotates triad. but the r-axis is adjusted to lie along the line between the two beam nodal points. This option is not recommended for zero length discrete beams. EQ.+3.0: beam node 2, the angular velocity of node 2 rotates triad. EQ.+12.0: Like +2.0, but with correction for beam rotation EQ.+13.0: Like +3.0, but with correction for beam rotation Nonstructural mass per unit length. This option applies to beam types 1-5 and does not apply to discrete, 2D, and spotweld beams, respectively. Beam thickness (CST = 0.0, 2.0) or outer diameter (CST = 1.0) in s direction at node 𝑛!. Note that the thickness defined on the *ELE- MENT_BEAM_THICKNESS card overrides the definition give here. Thickness at node 𝑛1 for beam formulations 7 and 8. Beam thickness (CST = 0.0, 2.0) or outer diameter (CST = 1.0) in s direction at node 𝑛2. For truss elements only, it is the ramp up time for the stress initialization by dynamic relaxation. Thickness at node 𝑛2 for beam formulations 7 and 8. NSM TS1 TS2 VARIABLE DESCRIPTION TT1 TT2 Beam thickness (CST = 0.0, 2.0) or inner diameter (CST = 1.0) in t direction at node 𝑛1. For truss elements only, it is the stress for the initialization of the stress by dynamic relaxation. Not used by beam formulations 7 and 8. Beam thickness (CST = 0.0, 2.0) or inner diameter (CST = 1.0) in t direction at node 𝑛2. Not used by beam formulations 7 and 8. NSLOC Location of reference surface normal to 𝑠 axis for Hughes-Liu beam elements only. See Remark 5. EQ.1.0: side at 𝑠 = 1.0, EQ.0.0: center, EQ.-1.0: side at 𝑠 = −1.0. NTLOC Location of reference surface normal to 𝑡 axis for Hughes-Liu beam elements only. See Remark 5. EQ.1.0: side at 𝑡 = 1.0, EQ.0.0: center, EQ.-1.0: side at 𝑡 = −1.0. A ISS ITT J SA Cross-sectional area. The definition on *ELEMENT_BEAM_- THICKNESS overrides the value defined here. 𝐼𝑠𝑠, area moment of inertia about local 𝑠-axis. The definition on *ELEMENT_BEAM_THICKNESS overrides the value defined here. 𝐼𝑡𝑡, area moment of inertia about local 𝑡-axis. The definition on *ELEMENT_BEAM_THICKNESS overrides the value defined here. 𝐽, torsional constant. The definition on *ELEMENT_BEAM_ THICKNESS overrides the value defined here If J is zero, then J is reset to the sum of ISS + ITT as an approximation for warped beam. Shear area. The definition on *ELEMENT_BEAM_THICKNESS overrides the value defined here. VARIABLE DESCRIPTION IST YS ZS IYR IZR IRR IW IWR PR 𝐼𝑠𝑡, product area moment of inertia w.r.t. local 𝑠- and 𝑡-axis. This is only non-zero for asymmetric cross sections and it can take positive and negative values, e.g. it is negative for SECTION_03. 𝑠 coordinate of shear center of cross-section. (The coordinate system is located at the centroid.) 𝑡 coordinate of shear center of cross-section. (The coordinate system is located at the centroid.) ∫ 𝑠𝑟2𝑑𝐴 , where 𝑟2 = 𝑠2 + 𝑡2 ∫ 𝑡𝑟2𝑑𝐴 , where 𝑟2 = 𝑠2 + 𝑡2 ∫ 𝑟4𝑑𝐴 , where 𝑟2 = 𝑠2 + 𝑡2 Warping constant. ∫ 𝜔2𝑑𝐴 , where 𝜔 is the sectorial area. ∫ 𝜔𝑟2𝑑𝐴 Pressure inside ELBOW elements that belong to the section. The pressure acts as a stiffener and will reduce the ovalization of the pipe. Pressure acting on the inside wall is taken as positive. IOVPR Print flag for the ELBOW ovalization degrees of freedom. EQ.1.0: an ascii file named elbwov is created and filled with the ovalization. Default no file is created. IPRSTR Flag for adding stress due to pressure PR into the material routine. EQ.0: No stress is added to the material. In this case the pressure only acts as a stiffener for the tube. EQ.1: The pressure PR is used to calculate additional axial and circumferential stresses due to the applied pressure PR. The stress added is given by: 𝜎axial = PR × 4𝑇 , 𝜎circ = pr × 2𝑇 for a straight pipe, and 𝜎axial = PR × 4𝑇 , 𝜎circ = PR × 4𝑇 [2𝑅 + 𝑟 cos(𝜃)] [𝑅 + 𝑟 cos(𝜃)] for a curved pipe. D is the pipe diameter, T is the thickness, R is VARIABLE DESCRIPTION RAMPT STRESS the curvature of the bend, r is the pipe radius (mean) and θ is an angle pointing out a point on the pipe. EQ.1 also includes the stiffening effect. Optional ramp-up time for dynamic relaxation. At the end of the ramp-up time, a uniform stress, STRESS, will exist in the truss in the truss element. This option will not work for hyperelastic materials. Optional initial stress for dynamic relaxation. At the end of dynamic relaxation a uniform stress equal to this value should exist in the truss element. STYPE Section type (A format) of resultant beam, see Figure 36-1: EQ.SECTION_01: I-Shape EQ.SECTION_02: Channel EQ.SECTION_03: L-shape EQ.SECTION_04: T-shape EQ.SECTION_05: Tubular box EQ.SECTION_06: Z-Shape EQ.SECTION_07: Trapezoidal EQ.SECTION_08: Circular EQ.SECTION_09: Tubular EQ.SECTION_10: I-Shape 2 EQ.SECTION_11: Solid Box EQ.SECTION_12: Cross EQ.SECTION_13: H-Shape EQ.SECTION_14: T-Shape 2 EQ.SECTION_15: I-Shape 3 EQ.SECTION_16: Channel 2 EQ.SECTION_17: Channel 3 EQ.SECTION_18: T-Shape 3 EQ.SECTION_19: Box-Shape 2 EQ.SECTION_20: Hexagon EQ.SECTION_21: Hat-Shape EQ.SECTION_22: Hat-Shape 2 D1-D6 Input parameters for section option using STYPE above. VOL Volume of discrete beam and scalar (MAT_146) beam. Used in calculating mass. If VOL = 0 for cable elements, volume is calculated as the product of cable length and cable area. If the mass density of the material model for the discrete beam is set to unity, the magnitude of the lumped mass can be defined here instead. This lumped mass is partitioned to the two nodes of the beam element. The translational time step size for the type 6 beam is dependent on the volume, mass density, and the translational stiffness values, so it is important to define this parameter. Defining the volume is also essential for mass scaling if the type 6 beam controls the time step size. INER CID CA OFFSET *SECTION DESCRIPTION Mass moment of inertia for the six degree of freedom discrete beam and scalar (MAT_146) beam. This parameter does not apply to cable elements. This lumped inertia is partitioned to the two nodes of the beam element. The rotational time step size for the type 6 beam is dependent on the lumped inertia and the rotational stiffness values, so it is important to define this parameter if the rotational springs are active. Defining the rotational inertia is also essential for mass scaling if the type 6 beam rotational stiffness controls the time step size. It is recommended to always set this parameter to a reasonable nonzero value to avoid instabilities and/or having model dependent rotational inertia properties, if the value set is smaller than that of an equivalent solid sphere LS-DYNA will issue a warning. Coordinate system ID for orientation (material types 66-69, 93, 95, 97), see *DEFINE_COORDINATE_option. If CID = 0, a default coordinate system is defined in the global system or on the third node of the beam, which is used for orientation. This option is not defined for material types than act between two nodal points, such as cable elements. The coordinate system rotates with the discrete beam, see SCOOR above. Cable area. See material type 71, *MAT_CABLE_DISCRETE_- BEAM. Optional offset for cable. See material type 71, *MAT_CABLE_- DISCRETE_BEAM. RRCON 𝑟-rotational constraint for local coordinate system EQ.0.0: Coordinate ID rotates about 𝑟 axis with nodes. EQ.1.0: Rotation is constrained about the 𝑟-axis SRCON 𝑠-rotational constraint for local coordinate system EQ.0.0: Coordinate ID rotates about 𝑠 axis with nodes. EQ.1.0: Rotation is constrained about the 𝑠-axis TRCON 𝑡-rotational constraint for local coordinate system EQ.0.0: Coordinate ID rotates about 𝑡 axis with nodes. EQ.1.0: Rotation is constrained about the 𝑡-axis CID *SECTION_BEAM DESCRIPTION Coordinate system ID for orientation, material type 146, see *DE- FINE_COORDINATE_SYSTEM. If CID = 0, a default coordinate system is defined in the global system. DOFN1 Active degree-of-freedom at node 1, a number between 1 and 6 where 1 in 𝑥-translation and 4 is 𝑥-rotation. DOFN2 Active degree-of-freedom at node 2, a number between 1 and 6. PRINT Output spot force resultant from spotwelds. EQ.0.0: Data is output to swforc file. EQ.1.0: Output is suppressed. Remarks: 1. Implicit Time Integrator. For implicit calculations all of the beam element choices are implemented: 2. Truss Elements. For the truss element, define the cross-sectional area, 𝐴, only. 3. Local Coordinate System Rotation. The local coordinate system rotates as the nodal points that define the beam rotate. In some cases this may lead to unexpected results if the nodes undergo significant rotational motions. In the definition of the local coordinate system using *DEFINE_COORDINATE_- NODES, if the option to update the system each cycle is active then this updat- ed system is used. This latter technique seems to be more stable in some applications. 4. Integrated Warped Beam. The integrated warped beam (type 11) is a 7 degree of freedom beam that must be used with an integration rule of the open stand- ard cross sections, see *INTEGRATION_BEAM. To incorporate the additional degrees of freedom corresponding to the twist rates, the user should declare one scalar node (*NODE_SCALAR) for each node attached to a warped beam. This degree of freedom is associated to the beam element using the warpage option on the *ELEMENT_BEAM card. 5. Beam Offsets. Beam offsets are sometimes necessary for correctly modeling beams that act compositely with other elements such as shells or other beams. A beam offset extends from the beam’s 𝑛1-to-𝑛2 axis to the reference axis of the beam. The beam reference axis lies at the origin of the local 𝑠 and 𝑡 axes. This origin is located at the center of the cross-section footprint for beam formula- tions 1 and 11 but it is located at the cross-section centroid for beam formula- tion 2. Note that for cross-sections that are not doubly symmetric, e.g, a T- section, the center of the cross-section footprint and the centroid of the cross- section do not coincide. The offset in the positive 𝑠-direction is s-offset = −0.5 × NSLOC × (beam cross-section dimension in 𝑠-direction). Similarly, the offset in the positive t-direction is t-offset = −0.5 × NTLOC × (beam cross-section dimension in 𝑡-direction). If IRID is used to point to an integration rule with ICST > 0, then offsets must be defined using SREF and TREF on the *INTEGRATION_BEAM card as they will override NSLOC and NTLOC even if SREF = 0 or TREF = 0. See also *ELEMENT_BEAM_OFFSET for an alternate approach to defining beam offsets. 6. 3-D Timoshenko Beam. Element type 13 is a 3-D Timoshenko resultant-based beam element with two nodes for small displacement, linear isotropic elasticity. The stiffness matrix is identical to the residual stiffness formulation used in the Belytschko-Schwer element (type 2). This element only works with *MAT_- ELASTIC. It uses the reference geometry to calculate the element stiffness and calculates the element forces by multiplying the element stiffness by the dis- placements. Offsets work but they are fixed for all time like the reference ge- ometry. 7. SCOOR. If the magnitude of SCOOR is less than or equal to unity then zero length discrete beams are assumed with infinitesimal separation between the nodes in the deformed state. For large separations or nonzero length beams set |SCOOR| to 2, 3, 12, or 13, in which case true beam-like behavior is invoked to provide equilibrating torques to offset any force couples that arise due to trans- lational stiffness or translational damping. Also, rigid body rotation is meas- ured and the spring strain modified so that rotation does not create strain. A flaw in this strain modification was found in the implementation of |SCOOR| = 2 and 3 the improved formulation is activated by setting |SCOOR| = 12 and 13. The original options were left in place to allow legacy data to run without change. 8. Disabling Nodal Rotations. RRCON, SRCON, and TRCON are optional and apply only to non-cable discrete beams. If set to 1, RRCON, SRCON, and TRCON will prevent nodal rotations about the local 𝑟, 𝑠, 𝑡 axes, respectively, from affecting the update of the local coordinate system. These three parame- ters have no influence on how nodal translations may affect the local coordinate system update. 9. Note about Local Coordinate Updates and FLAG. If CID is nonzero for a discrete beam and the coordinate system identified by CID uses *DEFINE_CO- ORDINATE_NODES with FLAG=1, the beam local system is updated based on the current orientation of the three nodes identified in *DEFINE_COORDI- NATE_NODES. In this case, local coordinate system updates per SCOOR types 0, ±1, ±3, and ±13 are inactive while for SCOOR types ±2 and ±12, a final adjustment is made to the local coordinate system so that the local 𝑟-axis lies along the 𝑛1-to-𝑛2 axis of the beam. An optional output database (*DATA- BASE_DISBOUT) will report relative displacements, rotations, and force result- ants of discrete beams, all in the local coordinate system. 10. Beams 7 and 8. Beam formulations 7 and 8 are 2D shell elements. For these two formulations, variable QR/IRID is the number of through thickness inte- gration points for the shell. Output for these integration points is controlled by the variable BEAMIP in *DATABASE_EXTENT_BINARY. $$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ $ $$$$ *SECTION_BEAM $ $$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ $ $ Define a Belytschko-Schwer resultant beam (elform = 2) with the following $ properties. This beam models the connection/stiffening beams of a medium $ size roadside sign. $ $ cross sectional area: a = 515.6 mm2 $ 2nd moment of area about s-axis: iss = 99,660.0 mm4 $ 2nd moment of area about t-axis: iss = 70,500.0 mm4 $ 2nd polar moment of area about beam axis: j = 170,000.0 mm4 $ *SECTION_BEAM $ $...>....1....>....2....>....3....>....4....>....5....>....6....>....7....>....8 $ sid elform shrf qr/irid cst 111 2 $ $ a iss itt j sa 515.6 99660.0 70500.0 170000.0 $ *SECTION_BEAM_TITLE Main beam member $ $...>....1....>....2....>....3....>....4....>....5....>....6....>....7....>....8 $ sid elform shrf qr/irid cst 111 2 $ $ a iss itt j sa 515.6 99660.0 70500.0 170000.0 $ $$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ D3 D2 D4 D1 D4 D3 D1 D2 Figure 36-1. SECTION_01 ⇒ I-Shape Figure 36-2. SECTION_02 ⇒ Channel D4 D3 D1 D2 D3 D1 D2 D4 Figure 36-3. SECTION_03 ⇒ L-Shape Figure 36-4. SECTION_04 ⇒ T-Shape D3 D2 D1 D4 D1 D4 D3 D2 Figure 36-5. SECTION_05 ⇒ Box-Shape Figure 36-6. SECTION_06 ⇒ Z-Shape D1 D3 D2 D1 Figure 36-7. SECTION_07 ⇒ Trapezoidal- Figure 36-8. SECTION_08 ⇒ Circular Shape D1 D2 D6 D5 D3 D2 D4 D1 Figure 36-9. SECTION_09 ⇒ Tubular Figure 36-10. SECTION_10 ⇒ I-Shape 2 D2 D1 D4 D3 D1/2 D1/2 D2 Figure 36-11. SECTION_11 ⇒ Solid Box Figure 36-12. SECTION_12 ⇒ Cross D2/2 D4 D2/2 D3 D4 D3 D1 D2 D1 Figure 36-13. SECTION_13 ⇒ H-Shape Figure 36-14. SECTION_14 ⇒ T-Shape 2 D1/2 D4 D2 D1/2 D3 D4 D1 D3 D2 Figure 36-15. SECTION_15 ⇒ I-Shape 3 Figure 36-16. SECTION_16 ⇒ Channel 2 D1 D3 D1 D2 D4 D2 D4 D1 D3 Figure 36-17. SECTION_17 ⇒ Channel 3 Figure 36-18. SECTION_18 ⇒ T-Shape 3 D1 D2 D5 D3 D6 D2 D3 D4 D1 Figure 36-19. SECTION_19 ⇒ Box-Shape Figure 36-20. SECTION_20 ⇒ Hexagon 2 D3 D1 D4 D2 D4 Figure 36-21. SECTION_21 ⇒ Hat Shape D2 D6 D4 D3 D1 D6 D5 Figure 36-22. SECTION_22 ⇒ Hat Shape 2 *SECTION_BEAM_AISC Purpose: Define cross-sectional properties for beams and trusses using section labels from the AISC Steel Construction Manual, 2005, 13th Edition, as published in the AISC Shapes Database V13.1.1 Card Sets. For each BEAM_AISC section include one pair of cards 1 and 2. This input ends at the next keyword (“*”) card. Card 1 1 2 3 4 5 6 7 8 Variable SECID Type I LABEL A70 Integrated Beam Card (types 1 and 11). Card 2 for ELFORM equal to 1 or 11. Card 2 1 2 3 4 5 6 Variable ELFORM SHRF NSM LFAC NSLOC NTLOC Type I F F F F F 8 7 K I Resultant Beam Card (types 2 and 12). Card 2 for ELFORM equal to 2 or 12. Card 2 1 2 3 4 5 6 7 8 Variable ELFORM SHRF NSM LFAC Type I F F F Truss Beam Card (type 3). Card 2 for ELFORM equal to 3. Card 2 1 2 3 4 5 6 7 8 Variable ELFORM LFAC RAMPT STRESS Type I F F Integrated Beam Card (types 4 and 5). Card 2 for ELFORM equal to 4 or 5. Card 2 1 2 3 4 Variable ELFORM SHRF NSM LFAC 5 K 6 7 8 Type I F F K VARIABLE SECID DESCRIPTION Section ID. SECID is referenced on the *PART card. A unique number or label must be specified. LABEL AISC section label ELFORM Element formulation . Only types 1– 5,11,12 are allowed SHRF NSM LFAC Shear factor Non-structural mass per unit length GT.0.0: Length scale factor to convert dimensions from standard units LT.0.0: Use predefined length factor for specific model units EQ.-1.0: ft EQ.-2.0: m EQ.-3.0: in EQ.-4.0: mm EQ.-5.0: cm NSLOC Location of reference surface NTLOC Location of reference surface K Integration refinement parameter RAMPT Optional ramp-up time STRESS Optional initial stress *SECTION_BEAM_AISC This keyword uses the dimensions of the standard AISC beams sections — as defined by the section label — to define *SECTION_BEAM and *INTEGRATION_BEAM cards with the appropriate parameters. The AISC section label may be specified either as the shape designation as seen in the AISC Steel Construction Manual, 2005, or the designation according to the AISC Naming Convention for Structural Steel Products for Use in Electronic Data Interchange (EDI), 2001. As per the EDI convention, the section labels are to be case-sensitive and space sensitive, i.e. “W36X150” is acceptable but “W36 x 150” is not. Labels can be specified in terms of either the U.S. Customary units (in) or metric units (mm), which will determine the length units for the section dimensions. The parameter LFAC may be used as a multiplier to convert the dimensions to other lengths units. For user convenience, predefined conversion factors are provided for specific choices of the model length unit. AISC requires the following legal notice specifying that LS-DYNA users may not extract AISC shapes data in any manner from LS-DYNA to create commercial software. Users are certainly allowed to create LS-DYNA input models for commercial purposes using this card. AISC FLOW-DOWN LICENSE TERMS (TERMS OF USE) This application contains software from the American Institute of Steel Construction, Inc. of Chicago, Illinois d/b/a AISC (“AISC”). The software from AISC (the “AISC Shapes Database”) enables this application to provide dimensions and properties of structural steel shapes and to perform other functions. You may use AISC Data only by means of the intended End User functions of this application software. You agree that you will use AISC Data for non-commercial use only, meaning that it will not be used to develop or create revenue-producing software. You agree not to assign, copy, transfer or transmit the AISC Shapes Database or any AISC Data to any third party. YOU AGREE NOT TO USE OR EXPLOIT AISC DATA OR THE AISC SHAPES DATABASE EXCEPT AS EXPRESSLY PERMITTED HEREIN. *SECTION Purpose: Defined spring and damper elements for translation and rotation. These definitions must correspond with the material type selection for the elements, i.e., *MAT_SPRING_... and *MAT_DAMPER_... Card Sets. For each DISCRETE section include a pair of cards 1 and 2. This input ends at the next keyword (“*”) card. 3 KD F 3 4 V0 F 4 5 CL F 5 6 FD F 6 7 8 7 8 Card 1 1 2 Variable SECID DRO Type I/A Card 2 1 I 2 Variable CDL TDL Type F F VARIABLE SECID DESCRIPTION Section ID. SECID is referenced on the *PART card. A unique number or label must be specified. DRO Displacement/Rotation Option: EQ.0: the material describes a translational spring/damper, EQ.1: the material describes a torsional spring/damper. Dynamic magnification factor. See Remarks 1 and 2 below. Test velocity Clearance. See Remark 3 below. Failure deflection (twist for DRO = 1). Negative for compression, positive for tension. Deflection (twist for DRO = 1) limit in compression. See Remark 4 below. KD V0 CL FD CDL Deflection (twist for DRO = 1) limit in tension. See Remark 4 below. *SECTION VARIABLE TDL Remarks: 1. The constants from KD to TDL are optional and do not need to be defined. 2. If kd is nonzero, the forces computed from the spring elements are assumed to be the static values and are scaled by an amplification factor to obtain the dy- namic value: 𝐹dynamic = (1. +𝑘𝑑 𝑉0 ) 𝐹static where V = absolute value of the relative velocity between the nodes. V0 = dynamic test velocity. For example, if it is known that a component shows a dynamic crush force at 15m/s equal to 2.5 times the static crush force, use kd = 1.5 and V0 = 15. 3. Here, “clearance” defines a compressive displacement which the spring sustains before beginning the force-displacement relation given by the load curve defined in the material selection. If a non-zero clearance is defined, the spring is compressive only. 4. The deflection limit in compression and tension is restricted in its application to no more than one spring per node subject to this limit, and to deformable bod- ies only. For example in the former case, if three springs are in series, either the center spring or the two end springs may be subject to a limit, but not all three. When the limiting deflection is reached, momentum conservation calculations are performed and a common acceleration is computed in the appropriate di- rection. An error termination will occur if a rigid body node is used in a spring definition where deflection is limited. Constrained boundary conditions on the *NODE cards and the BOUNDARY_- SPC cards must not be used for nodes of springs with deflection limits. 5. Discrete elements can be included in implicit applications. $$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ $ $$$$ *SECTION_DISCRETE $ $$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ $ $ Note: These examples are in kg, mm, ms, kN units. $ $ A translational spring (dro = 0) is defined to have a failure deflection $ of 25.4 mm (fd = 25.4). The spring has no dynamic effects or $ deflection limits, thus, those parameters are not set. $ *SECTION_DISCRETE $ $...>....1....>....2....>....3....>....4....>....5....>....6....>....7....>....8 $ sid dro kd v0 cl fd 104 0 25.4 $ $ cdl tdl $ $ $ Define a translational spring that is known to have a dynamic crush force $ equal to 2.5 times the static force at a 15 mm/ms deflection rate. $ Additionally, the spring is known to be physically constrained to deflect $ a maximum of 12.5 mm in both tension and compression. $ *SECTION_DISCRETE $...>....1....>....2....>....3....>....4....>....5....>....6....>....7....>....8 $ sid dro kd v0 cl fd 107 0 1.5 15.0 $ $ cdl tdl 12.5 12.5 $ $$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ *SECTION_POINT_SOURCE Purpose: This command provides the inlet boundary condition for single gas in flow (inflation potential) via a set of point source(s). It also provides the inflator orifice geometry information. It requires 3 curves defining the inlet condition for the inflator gas coming into the tank or an airbag as input (𝑇̅̅̅̅gas corrected(𝑡), 𝑣𝑟(𝑡), and vel(𝑡)). Please see also the *ALE_TANK_TEST card for additional information. Card 1 1 2 3 4 5 6 7 8 Variable SECID LCIDT LCIDVR LCIDVEL NIDLC1 NIDLC2 NIDLC3 Type I/A Default 0 I 0 I 0 I 0 I 0 I 0 I 0 Source Node Cards. Include one card for each source node. This input ends at the next keyword (“*”) card. Card 2 1 2 3 4 5 6 7 8 Variable NODEID VECID ORIFA Type Default I 0 I 0 F 0.0 VARIABLE DESCRIPTION SECID LCIDT Section ID. A unique number or label must be specified. Temperature load curve ID LCIDVR Relative volume load curve ID LCIDVEL Inlet flow velocity load curve ID NIDLC1 NIDLC2 The 1st node ID defining a local coordinate . The 2nd node ID defining a local coordinate . VARIABLE DESCRIPTION NIDLC3 The 3rd node ID defining a local coordinate . NODEID The node ID(s) defining the point source(s). VECID The vector ID defining the direction of flow at each point source. ORIFA The orifice area at each point source. Remarks: 1. 2. In an airbag inflator tank test, the tank pressure data is measured. This pressure is used to derive 𝑚̇ (𝑡) and the estimated 𝑇̅̅̅̅𝑔𝑎𝑠(𝑡), usually via a lumped- parameter method, a system of conservation equations and EOS. Subsequently 𝑚̇ (𝑡) and 𝑇̅̅̅̅𝑔𝑎𝑠(𝑡) (stagnation temperature) are used as input to obtain 𝑇̅̅̅̅𝑔𝑎𝑠_ 𝑐𝑜𝑟𝑟𝑒𝑐𝑡𝑒𝑑(𝑡) (static temperature), 𝑣𝑟(𝑡), and 𝑣𝑒𝑙(𝑡). These 3 curves are then used to describe inflator gas inlet condition . In a car crash model, the inflator housing may get displaced during the impact. The 3 node IDs defines the local reference coordinate system to which the point sources are attached. These 3 reference nodes may be located on a rigid body which can translate and rotate as the inflator moves during the impact. This allows for the point sources to move in time. These reference nodes may be used as the point sources themselves. 3. If the *ALE_TANK_TEST card is present, please see the Remarks under that card. Example: Consider a tank test model which consists of the inflator gas (PID 1) and the air inside the tank (PID 2). The 3 load curves define the thermodynamic and kinetic condition of the incoming gas. The nodes define the center of the orifice, and the vector the direction of flow at each orifice. $...|....1....|....2....|....3....|....4....|....5....|....6....|....7....|...8 *PART inflator gas $ PID SECID MID EOSID HGID GRAV ADPOPT TMID 1 1 1 0 0 0 0 0 *SECTION_POINT_SOURCE $ SECID LCIDT LCIDVOLR LCIDVEL NIDLCOOR1 NIDLCOOR2 NIDLCOOR3 1 3 4 5 0 0 0 $ NODEID VECTID AREA 24485 3 15.066 ... 24557 3 15.066 *PART air inside the tank $ PID SECID MID EOSID HGID GRAV ADPOPT TMID 2 2 2 0 0 0 0 0 *SECTION_SOLID $ SECID ELFORM AET 2 11 0 *ALE_MULTI-MATERIAL_GROUP $ SID SIDTYPE 1 1 2 1 $...|....1....|....2....|....3....|....4....|....5....|....6....|....7....|...8 *SECTION_POINT_SOURCE_MIXTURE Purpose: This command provides (a) an element formulation for a solid ALE part of the type similar to ELFORM = 11 of *SECTION_SOLID, and (b) the inlet gas injection boundary condition for multiple-gas mixture in-flow via a set of point source(s). It also provides the inflator orifice geometry information. This must be used in combination with the *MAT_GAS_MIXTURE and/or *INITIAL_GAS_MIXTURE card . Card 1 1 2 3 4 5 6 7 8 Variable SECID LCIDT Not Used LCIDVEL NIDLC1 NIDLC2 NIDLC3 IDIR Type I/A I I I I I Default none none none none none none Card 2 1 2 3 4 5 6 7 I 0 8 Variable LCMD1 LCMD2 LCMD3 LCMD4 LCMD5 LCMD6 LCMD7 LCMD8 Type I I I I I I I I Default none none none none none none none none Source Node Cards. Include one card for each source node. This input ends at the next keyword (“*”) card. Card 3 1 2 3 4 5 6 7 8 Variable NODEID VECID ORIFA Type I I F Default none none 0.0 VARIABLE DESCRIPTION SECID Section ID. A unique number or label must be specified. LCIDT *SECTION_POINT_SOURCE_MIXTURE DESCRIPTION Inflator gas mixture average stagnation temperature load curve ID (all gases of the mixture are assumed to have the same average temperature). LCIDVEL User-defined inflator gas mixture average velocity load curve ID. If LCIDVEL = 0 or blank, LSDYNA will estimate the inlet gas velocity. NIDLC001 The 1st node ID defining a local coordinate . NIDLC002 The 2nd node ID defining a local coordinate . NIDLC003 The 3rd node ID defining a local coordinate . IDIR A flag for constraining the nodal velocity of the nodes of the ALE element containing a point source. If IDIR = 0 (default), then the ALE nodes behind the point source (relative position of nodes based on the vector direction of flow of point source) will have zero velocity. If IDIR = 1, then all ALE nodes will have velocity distributed based on energy conservation. The latter option seems to be more robust in airbag modeling . LCMD1 LCMDn LCMD8 The mass flow rate load curve ID of the1st gas in the mixture. The mass flow rate load curve ID of the nth gas in the mixture. The mass flow rate load curve ID of the 8th gas in the mixture. NODEID The node ID(s) defining the point sources . VECID The vector ID defining the direction of flow at each point source. ORIFA The orifice area at each point source. Remarks: 1. This command is used to define a part that acts as the ideal gas mixture injection source. The associated ALE material (gas mixture) may not be present at time zero, but can be introduced (injected) into an existing ALE domain. For airbag application, the input from control volume analysis, inlet mass flow rate, 𝑚̇ (𝑡), and, inlet stagnation gas temperature, 𝑇̅̅̅̅𝑔𝑎𝑠(𝑡) may be used as direct input for ALE analysis. If available, the user may input a load curve for the gas mix- ture average inlet velocity. If not, LS-DYNA will estimate the inlet gas velocity. 2. The gas mixture is assumed to have a uniform temperature (𝑇̅̅̅̅ ≈ 𝑇𝑖) and inlet velocity. However, the species in the mixture may each have a different inlet mass flow rate. 3. A brief review of the concept used is presented. The total energy (𝑒𝑇) is the sum of internal (𝑒𝑖) and kinetic (𝑉2 2 ) energies, (per unit mass). 𝑒𝑇 = 𝑒𝑖 + 𝑉2 𝐶𝑉𝑇𝑠𝑡𝑎𝑔 = 𝐶𝑉𝑇 + 𝑉2 𝑇𝑠𝑡𝑎𝑔 = 𝑇 + 𝑉2 2𝐶𝑉 The distinction between stagnation and static temperatures is shown above. 𝐶𝑉 is the constant-volume heat capacity. The gas mixture average internal energy per unit mass in terms of mixture species contribution is 𝜌𝑖 𝜌𝑚𝑖𝑥𝑡𝑢𝑟𝑒 ) 𝐶𝑉𝑖𝑇𝑖 = [∑ ( 𝜌𝑖 𝜌𝑚𝑖𝑥𝑡𝑢𝑟𝑒 ) 𝐶𝑉𝑖 ] 𝑇̅̅̅̅ 𝑒𝑖 = 𝐶̅𝑉𝑇̅̅̅̅ = ∑ ( 𝐶̅𝑉 = [∑ ( 𝜌𝑖 𝜌𝑚𝑖𝑥𝑡𝑢𝑟𝑒 ) 𝐶𝑉𝑖 ] Since we approximate 𝑇̅̅̅̅ ≈ 𝑇𝑖, then gas mixture average static temperature is related to the mixture average internal energy per unit mass as following 𝑇̅̅̅̅ = 𝑒𝑖 𝜌𝑖 𝜌𝑚𝑖𝑥𝑡𝑢𝑟𝑒 [∑ ( )𝐶𝑉𝑖 ] Note that the “i” subscript under “e” denotes “internal” energy, while the other “i” subscripts denote the “ith” species in the gas mixture. The total mixture pressure is the sum of the partial pressures of the individual species. 𝑝̅ = ∑ 𝑝𝑖 The ideal gas EOS applies to each individual species (by default) 𝑃𝑖 = 𝜌𝑖(𝐶𝑃𝑖 − 𝐶𝑉𝑖)𝑇𝑖 4. Generally, it is not possible to conserve both momentum and kinetic (KE) at the same time. Typically, internal energy (IE) is conserved and KE may not be. This may result in some KE loss (hence, total energy loss). For many analyses this is tolerable, but for airbag application, this may lead to the reduction of the inflating potential of the inflator gas. In *MAT_GAS_MIXTURE computation, any kinetic energy not accounted-for during advection is stored in the internal energy. Therefore, there is no kinetic energy loss, and the total energy of the element is conserved over the advection step. This is a simple, ad hoc approach that is not rigorously derived for the whole system based on first principles. Therefore it is not guaranteed to apply universally to all scenarios. It is the user’s responsibility to validate the model with data. 5. Since ideal gas is assumed, there is no need to define the EOS for the gases in the mixture. 6. In general, it is best to locate a point source near the center of an ALE element. Associated with each point source is an area and a vector indicating flow direc- tion. Each point source should occupy 1 ALE element by itself, and there should be at least 2 empty ALE elements between any 2 point sources. A point source should be located at least 3 elements away from the free surface of an ALE mesh for stability. Example 1: Consider a tank test model without coupling which consists of: -a background mesh with air (PID 1 = gas 1) initially inside that mesh (tank space), and -the inflator gas mixture (PID 2 consisting of inflator gases 2, 3, and 4). The mixture is represented by one AMMGID and the air by another AMMGID. The tank internal space is simply modeled with an Eulerian mesh of the same volume. The Tank itself is not modeled thus no coupling is required. The inflator gases fill up this space mixing with the air initially inside the tank. The background air (gas 1) is included in the gas mixture definition in this case because that air will participate in the mixing process. Only include in the mixture those gases that actually undergo mixing (gases 1, 2, 3 and 4). Note that for an airbag model, the “outside” air should not be included in the mixture (it should be defined independent- ly) since it does not participate in the mixing inside the airbag. This is shown in the next example. The nodes define the center of the orifices, and the vectors define the directions of flow at these orifices. $...|....1....|....2....|....3....|....4....|....5....|....6....|....7....|....8 *PART Tank background mesh, initially filled with air, allows gas mixture to flow in. $ PID SECID MID EOSID HGID GRAV ADPOPT TMID 1 1 1 0 0 0 0 0 *SECTION_SOLID $ SECID ELFORM AET 1 11 0 $ The next card defines the properties of the gas species in the mixture. *MAT_GAS_MIXTURE $ MID 1 $ Cv1 Cv2 Cv3 Cv4 Cv5 Cv6 Cv7 Cv8 654.47 482.00 2038.30 774.64 0.0 0.0 0.0 0.0 $ Cp1 Cp2 Cp3 Cp4 Cp5 Cp6 Cp7 Cp8 941.32 666.67 2500.00 1071.40 0.0 0.0 0.0 0.0 $ The next card specifies that gas 1 (background air) occupies PID 1 at time 0. *INTIAL_GAS_MIXTURE $ SID STYPE AMMGID TEMP0 1 1 1 293.00 $ RHO1 RHO2 RHO3 RHO4 RHO5 RHO6 RHO7 RHO8 1.20E-9 0.0 0.0 0.0 0.0 0.0 0.0 0.0 *PART The gas mixture (inlet) definition (no initial mesh required for this PID) $ PID SECID MID EOSID HGID GRAV ADPOPT TMID 2 2 1 0 0 0 0 0 *SECTION_POINT_SOURCE_MIXTURE $ SECID LCIDT NOTUSED LCIDVEL NIDLCOOR1 NIDLCOOR2 NIDLCOOR3 IDIR 2 1 0 5 0 0 0 0 $ LCMDOT1 LCMDOT2 LCMDOT3 LCMDOT4 LCMDOT5 LCMDOT6 LCMDOT7 LCMDOT8 0 2 3 4 0 0 0 0 $ NODEID VECTID AREA 24485 1 25.0 ... 24557 1 25.0 *ALE_MULTI-MATERIAL_GROUP $ SID SIDTYPE 1 1 2 1 *DEFINE_VECTOR $ VECTID XTAIL YTAIL ZTAIL XHEAD YHEAD ZHEAD 1 0.0 0.0 0.0 0.0 1.0 0.0 $...|....1....|....2....|....3....|....4....|....5....|....6....|....7....|....8 Example 2: Consider an airbag inflation model which consists of: -a background Eulerian mesh for air initially outside the airbag (PID 1) -the inflator gas mixture (PID 2 consisting of inflator gases 1, 2, and 3). The mixture is represented by one AMMGID and the air by another AMMGID. The background air (PID 1) is NOT included in the gas mixture definition in this case because that air will NOT participate in the mixing process. Only include in the mixture those gases that actually undergo mixing (gases 1, 2, and 3). Gases 1, 2, and 3 in this example correspond to gases 2, 3, and 4 in example 1. Compare the air properties in PID 1 here to that of example 1. Note that the *INITIAL_GAS_MIXTURE card is not required to initialize the background mesh in this case. $...|....1....|....2....|....3....|....4....|....5....|....6....|....7....|....8 *PART Tank background mesh, initially filled with air, allows gas mixture to flow in. $ PID SECID MID EOSID HGID GRAV ADPOPT TMID 1 1 1 0 0 0 0 0 *SECTION_SOLID $ SECID ELFORM AET 1 11 0 *MAT_NULL $ MID RHO PCUT MU TEROD CEROD YM PR 1 1.20E-9 -1.0E-6 0.0 0.0 0.0 0.0 0.0 *EOS_IDEAL_GAS $ EOSID CV0 CP0 COEF1 COEF2 T0 RELVOL0 1 654.47 941.32 0.0 0.0 293.00 1.0 $ The next card defines the properties of the gas species in the mixture. *PART The gas mixture (inlet) definition (no initial mesh required for this PID) $ PID SECID MID EOSID HGID GRAV ADPOPT TMID 2 2 2 0 0 0 0 0 *SECTION_POINT_SOURCE_MIXTURE $ SECID LCIDT NOTUSED LCIDVEL NIDLCOOR1 NIDLCOOR2 NIDLCOOR3 IDIR 2 1 0 5 0 0 0 0 $ LCMDOT1 LCMDOT2 LCMDOT3 LCMDOT4 LCMDOT5 LCMDOT6 LCMDOT7 LCMDOT8 2 3 4 0 0 0 0 0 $ NODEID VECTID AREA 24485 1 25.0 ... 24557 1 25.0 *MAT_GAS_MIXTURE $ MID 2 $ Cv1 Cv2 Cv3 Cv4 Cv5 Cv6 Cv7 Cv8 482.00 2038.30 774.64 0.0 0.0 0.0 0.0 $ Cp1 Cp2 Cp3 Cp4 Cp5 Cp6 Cp7 Cp8 666.67 2500.00 1071.40 0.0 0.0 0.0 0.0 $ The next card specifies that gas 1 (background air) occupies PID 1 at time 0. *ALE_MULTI-MATERIAL_GROUP $ SID SIDTYPE 1 1 2 1 *DEFINE_VECTOR $ VECTID XTAIL YTAIL ZTAIL XHEAD YHEAD ZHEAD 1 0.0 0.0 0.0 0.0 1.0 0.0 $...|....1....|....2....|....3....|....4....|....5....|....6....|....7....|....8 *SECTION Purpose: Define section properties for the seat belt elements. This card is required for the *PART Section. Currently, only the ID is required. Seatbelt Section Cards. Include one card for each SEATBELT section. This input ends at the next keyword (“*”) card. Card 1 1 2 3 4 5 6 7 8 Variable SECID AREA THICK Type I/A F F Default none 0.01 none VARIABLE DESCRIPTION Section ID. A unique number or label must be specified. Optional area of cross-section used in the calculation of contact stiffness, which is proportional to the cross-section area. Optional contact thickness which can be overwritten by a nonzero SST defined in *CONTACT. If not defined, a value proportional to element length is used as the contact thickness. SECID AREA THICK Remarks: Seatbelt elements are implemented for both explicit and implicit calculations. $$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ $ $$$$ *SECTION_SEATBELT $ $$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ $ $ Define a seat belt section that is referenced by part 10. Nothing $ more than the sid is required. $ *SECTION_SEATBELT $ $...>....1....>....2....>....3....>....4....>....5....>....6....>....7....>....8 $ sid 111 $ $ *PART Seatbelt material $...>....1....>....2....>....3....>....4....>....5....>....6....>....7....>....8 $ pid sid mid eosid hgid adpopt 10 111 220 $ $$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ *SECTION_SHELL_{OPTION} Available options include: <BLANK> EFG THERMAL XFEM Purpose: Define section properties for shell elements. Card Sets. For each shell section, of a type matching the keyword’s options, include one set data cards. This input ends at the next keyword (“*”) card. Card 1 1 2 3 4 5 6 7 8 Variable SECID ELFORM SHRF NIP PROPT QR / IRID ICOMP SETYP Type I/A I F Default none 1.0 Remarks Card 2 Variable 1 T1 Type F 1 2 T2 F 3 T3 F F 2 4 T4 F F F 0.0 0.0 I 0 I 1 5 6 7 8 NLOC MAREA IDOF EDGSET F F F I Default 0.0 T1 T1 T1 0.0 0.0 0.0 Remarks 6 Angle Cards. Additional cards for ICOMP = 1. Include the minimum number of cards necessary to input NIP values: 8 values per card ⇒ number of cards = ceil(NIP 8⁄ ) where ceil(𝑥) = the smallest integer greater than 𝑥. Card 3 Variable 1 B1 Type F 2 B2 F 3 B3 F 4 B4 F 5 B5 F 6 B6 F 7 B7 F 8 B8 F EFG Card. Additional card for EFG keyword option. See *CONTROL_EFG. Card 4 Variable 1 DX 2 3 4 5 6 7 8 DY ISPLINE IDILA IEBT IDIM Type F F Default 1.1 1.1 I 0 I 0 I I -1 or 1 2 or 1 Thermal Card. Additional Card for THERMAL keyword option. Card 4 1 2 3 4 5 6 7 8 Variable ITHELFM Type Default I 0 XFEM Card. Additional card for XFEM keyword option. See Remark 8. Card 4 1 2 3 4 5 Variable CMID BASELM DOMINT FAILCR PROPCR Type I I Default 36-42 (SECTION) I I 0 I 1 7 8 LS/FS1 NC/CL 6 FS User Defined Element Card. Additional card for ELFORM = 101,102,103,104 or 105. See Appendix C Card 5 1 2 3 4 5 6 7 8 Variable NIPP NXDOF IUNF IHGF ITAJ LMC NHSV ILOC Type Default I 0 I 0 I 0 I 0 I 0 I 0 I 0 I 0 User Defined Element Integration Point Cards. Additional cards for ELFORM = 101, 102, 103, 104 or 105. Define NIPP cards according to the following format. See Appendix C. Card 6 Variable Type 1 XI F 2 3 4 5 6 7 8 ETA WGT F F Default none none none User Defined Element Property Cards. Include the minimum number of cards necessary to input LMC values: 8 values per card ⇒ number of cards = ceil(LMC 8⁄ ) where ceil(𝑥) = the smallest integer greater than 𝑥. See Appendix C. Card 7 Variable Type Default 1 P1 F 0 2 P2 F 0 3 P3 F 0 4 P4 F 0 5 P5 F 0 6 P6 F 0 7 P7 F 0 8 P8 F 0 VARIABLE DESCRIPTION SECID Section ID. SECID is referenced on the *PART card. A unique VARIABLE DESCRIPTION number or label must be specified. ELFORM Element formulation options, see Remarks 1 and 2 below: EQ.1: EQ.2: EQ.3: EQ.4: EQ.5: EQ.6: EQ.7: EQ.8: EQ.9: EQ.10: EQ.11: Hughes-Liu, Belytschko-Tsay, BCIZ triangular shell, C0 triangular shell, Belytschko-Tsay membrane, S/R Hughes-Liu, S/R co-rotational Hughes-Liu, Belytschko-Leviathan shell, Fully integrated Belytschko-Tsay membrane, Belytschko-Wong-Chiang, Fast (co-rotational) Hughes-Liu, EQ.12: Plane stress (𝑥-𝑦 plane), EQ.13: Plane strain (𝑥-𝑦 plane), EQ.14: Axisymmetric solid (𝑥-𝑦 plane, 𝑦-axis of symmetry) - area weighted , EQ.15: Axisymmetric solid (𝑥-𝑦 plane, 𝑦-axis of symmetry) - volume weighted, EQ.16: Fully integrated shell element (very fast), EQ.-16: Fully integrated shell element modified for higher accuracy, see Remark 0. EQ.17: EQ.18: EQ.20: EQ.21: EQ.22: Fully integrated DKT, triangular shell element, Fully integrated linear DK quadrilateral/triangular shell Fully integrated linear assumed strain C0 shell . Fully integrated linear assumed strain C0 shell (5 DOF). Linear shear panel element. 3 DOF per node. . EQ.23: 8-node quadratic quadrilateral shell VARIABLE DESCRIPTION EQ.24: EQ.25: EQ.26: 6-node quadratic triangular shell Belytschko-Tsay shell with thickness stretch. Fully integrated shell with thickness stretch. EQ.27: C0 triangular shell with thickness stretch. EQ.29: Cohesive shell element for edge-to-edge connection of shells. See Remark 0. EQ.-29: Cohesive shell element for edge-to-edge connection of shells (more suitable for pure shear). See Remark 0. EQ.41: Mesh-free (EFG) shell local approach. (more suitable for crashworthiness analysis) EQ.42: Mesh-free (EFG) shell global approach. suitable for metal forming analysis) (more EQ.43: Mesh-free (EFG) plane strain formulation (𝑥-𝑦 plane). EQ.44: Mesh-free (EFG) axisymmetric solid formulation (𝑥-𝑦 plane, 𝑦-axis of symmetry). EQ.46: Cohesive element for two-dimensional plane strain, plane stress, and area-weighted axisymmetric prob- lems (type 14 shells). EQ.47: Cohesive element for two-dimensional volume- weighted axisymmetric problems (use with type 15 shells). EQ.52: EQ.54: EQ.55: Plane strain (𝑥-𝑦 plane) XFEM, base element type 13. Shell XFEM, base element type defined by BASELM (default 16). 8-node singular plane strain (𝑥-𝑦 plane) finite element, see Remark 11. EQ.98: Interpolation shell EQ.99: Simplified linear element for time-domain vibration studies. See Remark 4 below. EQ.101: User defined shell EQ.102: User defined shell EQ.103: User defined shell EQ.104: User defined shell VARIABLE DESCRIPTION EQ.105: User defined shell EQ.201: Isogeometric shells with NURBS. See *ELEMENT_SHELL_NURBS_PATCH GE.1000: Generalized shell element formulation (user defined). See *DEFINE_ELEMENT_GENERALIZED_SHELL The type 18 element is only for linear static and normal modes. It can also be used for linear springback in sheet metal stamping. For implicit modal computations element type 14 must be switched to type 15. Note that the 2D and 3D element types must not be mixed, and different types of 2D elements must not be used together. For example, 2D axisymmetric calculations can use either element types 14 or 15 but these element types must not be mixed together. Likewise, the plane strain element type must not be used with either the plane stress element or the axisymmetric element types. In 3D, the different shell elements types, i.e., 1-11 and 16, can be freely mixed together. Shear correction factor which scales the transverse shear stress. The shell formulations in LS-DYNA, with the exception of the BCIZ and DK elements, are based on a first order shear deformation theory that yields constant transverse shear strains which violates the condition of zero traction on the top and bottom surfaces of the shell. The shear correction factor is attempt to compensate for this error. A suggested value is 5/6 for isotropic materials. This value is incorrect for sandwich or laminated shells; consequently, laminated/sandwich shell theory is now an option in some of the constitutive models, e.g., material types 22, 54, and 55. Number of through thickness integration points. Either Gauss (default) or Lobatto integration can be used. The flag for Lobatto integration can be set on the control card, *CONTROL_SHELL. The location of the Gauss and Lobatto integration points are tabulated below. EQ.0.0: set to 2 integration points for shell elements. EQ.1.0: 1 point (no bending) EQ.2.0: 2 point EQ.3.0: 3 point SHRF NIP VARIABLE DESCRIPTION EQ.4.0: 4 point EQ.5.0: 5 point EQ.6.0: 6 point EQ.7.0: 7 point EQ.8.0: 8 point EQ.9.0: 9 point EQ.10.: 10 point GT.10.: trapezoidal or user defined rule Through thickness integration for the two-dimensional elements (options 12-15 above) is not meaningful; consequently, the default is equal to 1 integration point. Fully integrated two-dimensional elements are available for options 13 and 15 (but not 12 and 14) by setting NIP equal to a value of 4 corresponding to a 2 by 2 Gaussian quadrature. If NIP is 0 or 1 and the *MAT_SIMPLI- FIED_JOHNSON_COOK model then a resultant plasticity formulation is activated. NIP is always set to 1 if a constitutive model based on resultants is used. is used, PROPT Printout option (***NOT ACTIVE***): EQ.1.0: average resultants and fiber lengths, EQ.2.0: resultants at plan points and fiber lengths, EQ.3.0: resultants, stresses at all points, fiber lengths. QR/IRID Quadrature rule or Integration rule ID, see *INTEGRATION_- SHELL: ICOMP LT.0.0: absolute value is specified rule number, EQ.0.0: Gauss/Lobatto (up to 10 points are permitted), EQ.1.0: trapezoidal, not recommend for accuracy reasons. Flag for orthotropic/anisotropic layered composite material model. This option applies to material types 21, 22, 23, 33, 33_96, 34, 36, 40, 41-50, 54, 55, 58, 59, 103, 103_P, 104, 108, 116, 122, 133, 135, 135_PLC, 136, 157, 158, 190, 219, 226, 233, 234, 235, 242, and 243. For these material types, see *PART_COMPOSITE as an alternative to *SECTION_SHELL. Note: Please refer to Remark 5 under *MAT_034 for additional information specific to fiber directions for fabrics. VARIABLE DESCRIPTION EQ.1: a material angle in degrees is defined for each through thickness integration point. Thus, each layer has one integration point. SETYP Not used (obsolete). T1 T2 T3 T4 NLOC MAREA Shell thickness at node n1, unless the thickness is defined on the *ELEMENT_SHELL_OPTION card. Shell thickness at node n2, see comment for T1 above. Shell thickness at node n3, see comment for T1 above. Shell thickness at node n4, see comment for T1 above. Location of reference surface (shell mid-thickess) for three dimensional shell elements. If nonzero, the offset distance from the plane of the nodal points to the reference surface of the shell in the direction of the shell normal vector is a value, offset = −0.50 × NLOC × (average shell thickness). Except for Mortar contacts, this offset is not considered in the contact subroutines unless CNTCO is set to 1 in *CONTROL_- SHELL. Alternatively, the offset can be specified by using the OFFSET option in the *ELEMENT_SHELL input section. For Mortar contacts, NLOC or OFFSET determines the location of the contact surface regardless the value of CNTCO. EQ.1.0: nodes are located at top surface of shell, EQ.0.0: nodes are located at mid-thickness of shell (default), EQ.-1.0: nodes are located at bottom surface of shell. Non-structural mass per unit area. This is additional mass which comes from materials such as carpeting. This mass is not directly included in the time step calculation. Another and often more convenient alternative for defining distributed mass is by the option: *ELEMENT_MASS_PART, which allows additional non- structural mass to be distributed by an area weighted distribution to all nodes of a given part ID). IDOF Treatment of through thickess strain. LT.0: Same as IDOF.EQ.3 but the contact pressure is averaged over a time –IDOF in order to reduce noise and thus VARIABLE DESCRIPTION improve stability. EQ.1: The thickness field is continuous across the element edges for metalforming applications. This option applies to element types 25 and 26. EQ.2: The thickness field is discontinuous across the element edges. This is necessary for crashworthiness simulations due to shell intersections, sharp included angles, and non-smooth deformations. This option applies to ele- ment types 25, 26 and 27 and is mandatory for element 27. This is the default for these element types. EQ.3: The thickness strain is governed by the contact stress, meaning that the strain is adjusted for the through thick- ness stress to equilibrate the contact pressure. This op- tion applies to element types 2, 4, and ±16 . Edge node set required for shell type seatbelts. Input an ordered set of nodes along one of the transverse edges of a seatbelt. If there is no retractor associated with a belt, the node set can be on either edge. If the retractor exists, the edge must be on the retractor side and input in the same sequence of retractor node set. Therefore, another restriction on the seatbelt usage is that each belt has its own section definition and, therefore, a unique part ID. See Figure 17-16 in the section *ELEMENT_SEATBELT for additional clarification. 𝛽1, material angle at first integration point 𝛽2, material angle at second integration point 𝛽3, material angle at third integration point ⋮ 𝛽nip, material angle at NIPthintegration point. Normalized dilation parameters of the kernel function in X and Y directions. The normalized dilation parameters of the kernel function are introduced to provide the smoothness and compact support properties on the construction of the mesh-free shape functions. Values between 1.0 and 2.0 are recommended. Values smaller than 1.0 are not allowed. Larger values will increase the computation time and will sometimes result in a divergence problem. EDGSET B1 B2 B3 ⋮ BNIP DX, DY ISPLINE *SECTION_SHELL DESCRIPTION Replace the choice for the EFG kernel functions definition in *CONTROL_EFG. This allows users to define different ISPLINE in different sections. IDILA Replace the choice for the normalized dilation parameter definition in *CONTROL_EFG. This allows users to define different IDILA in different sections. IEBT Essential boundary condition treatment EQ.1: Full transformation (default for ELFORM = 42) EQ.-1: Without full transformation (default for ELFORM = 41) EQ.3: Coupled FEM/EFG EQ.7: Maximum entropy approximation IDIM For mesh-free shell local approach (ELFORM = 41) EQ.1: First-kind local boundary condition method EQ.2: Gauss integration (default) For mesh-free shell global approach (ELFORM = 42) EQ.1: First-kind local boundary condition method (default) EQ.2: Second-kind local boundary condition method ITHELFM Thermal shell formulation EQ.0: Default is governed by THSHEL on *CONTROL_SHELL EQ.1: Thick thermal shell EQ.2: Thin thermal shell CMID Cohesive material ID (only *MAT_COHESIVE_TH is available) BASELM Base element type for XFEM (type 13 for 2D, types 2 and 16 for shell) DOMINT Option for domain integration in XFEM: EQ.0: Phantom element integration EQ.1: Subdomain integration with triangular local boundary integration (available in 2D only) FAILCR Option for different failure criteria: VARIABLE DESCRIPTION EQ.1: Maximum tensile stress EQ.2: Maximum shear stress EQ.-1: Effective plastic strain EQ.-2: Crack length dependent EPS EQ.-n: n > 10, (n-10) points to HSVS for mat282/283 PROPCR Not used FS LS NC FS FS1 CL NIPP Failure strain/Failure critical value Length scale for strain regularization. > 0 activates regularization, available for FAILCR = -1 and –n for mat282/283 Number of cracks allowed in the part When FAILCR = -2, following three parameters represent : Initial failure plastic strain Final failure plastic strain Crack length failure strain reaches FS1 Number of in-plane integration points for user-defined shell (0 if resultant/discrete element) NXDOF Number of extra degrees of freedom per node for user-defined shell IUNF Flag for using nodal fiber vectors in user-defined shell: EQ.0: Nodal fiber vectors are not used. EQ.1: Nodal fiber vectors are used. IHGF Flag for using hourglass stabilization (NIPP.GT.0) EQ.0: Hourglass stabilization is not used EQ.1: LS-DYNA hourglass stabilization is used VARIABLE DESCRIPTION EQ.2: User-defined hourglass stabilization is used EQ.3: Same as 2, but the resultant material tangent moduli are passed ITAJ Flag for setting up finite element matrices (NIPP.GT.0) EQ.0: Set up matrices wrt isoparametric domain EQ.1: Set up matrices wrt physical domain LMC Number of property parameters NHSV Number of history variables ILOC Coordinate system option: EQ.0: Pass all variables in LS-DYNA local coordinate system EQ.1: Pass all variables in global coordinate system XI ETA WGT P1 P2 ⋮ First isoparametric coordinate Second isoparametric coordinate Isoparametric weight First user defined element property. Second user defined element property. ⋮ PLCM LCMth user defined element property. Gaussian Quadrature Points Point 1 Point 2 Points 3 Points 4 Points 5 Points #1 #2 #3 #4 #5 .0 -.5773503 .0 -.8611363 .0 +.5773503 -.7745967 -.3399810 -.9061798 +.7745967 +.3399810 -.5384693 +.8622363 +.5384693 +.9061798 Point 6 Points 7 Points 8 Points 9 Points 10 Points #1 #2 #3 #4 #5 #6 #7 #8 #9 #10 -.9324695 -.9491080 -.9702896 -.9681602 -.9739066 -.6612094 -.7415312 -.7966665 -.8360311 -.8650634 -.2386192 -.4058452 -.5255324 -.6133714 -.6794096 +.2386192 .0 -.1834346 -.3242534 -.4333954 +.6612094 +.4058452 +.1834346 .0 -.1488743 +.9324695 +.7415312 +.5255324 +.3242534 +.1488743 +.9491080 +.7966665 +.6133714 +.4333954 +.9702896 +.8360311 +.6794096 +.9681602 +.8650634 +.9739066 Location of through thickness Gauss integration points. The coordinate is referenced to the shell midsurface at location 0. The inner surface of the shell is at -1 and the outer surface is at +1. Lobatto Quadrature Points Point 1 Point 2 Points 3 Points 4 Points 5 Points #1 #2 #3 #4 #5 0.0 -1.0 +1.0 -1.0 0.0 -0.4472136 -1.0 +0.4472136 -0.6546537 +1.0 +0.6546537 +1.0 Point 6 Points 7 Points 8 Points 9 Points 10 Points #1 #2 #3 #4 #5 #6 #7 #8 #9 #10 -1.0 -1.0 -1.0 -1.0 -1.0 -0.7650553 -0.8302239 -0.8717401 -0.8997580 -0.9195339 -0.2852315 -0.4688488 -0.5917002 -0.6771863 -0.7387739 +0.2852315 0.0 -0.2092992 -0.3631175 -0.4779249 +0.7650553 +0.4688488 +0.2092992 0.0 -0.1652790 +1.0 +0.8302239 +0.5917002 +0.3631175 +0.1652790 +1.0 +0.8717401 +0.6771863 +0.4779249 +1.0 +0.8997580 +0.7387739 +1.0 +0.9195339 +1.0 Location of through thickness Lobatto integration points. The coordinate is referenced to the shell midsurface at location 0. The inner surface of the shell is at -1 and the outer surface is at +1. Remarks: 1. Formulation. The default shell formulation is 2 unless overridden by THEORY in *CONTROL_SHELL. ELFORM in *SECTION_SHELL overrides THEORY. For implicit calculations the following element formulations are implemented: 2, 5, 6, 10, 12,12, 13, 14, 15, 16, -16, 17, 18, 20, 21, 22, 23, 24, 25, 26, 27, 29, 41, 42, 55. If another element formulation is requested for an implicit analysis, LS-DYNA will substitute one of the above in place of the one chosen. 2. Linear Elements Type 18 and 20. The linear elements consist of an assembly of membrane and plate elements. They have six degrees of freedom per node and can, therefore, be connected to beams, or used in complex shell surface intersections. These elements possess the required zero energy rigid body modes and have exact constant strain and curvature representation, i.e. they pass all the first order patch tests. In addition, the elements have behavior approaching linear bending (cubic displacement) in the plate-bending configu- ration. a) The membrane component is based on an 8-node/6-node isoparametric mother element which incorporates nodal in-plane rotations through cu- bic displacement constraints of the sides [Taylor 1987; Wilson 2000]. b) The plate component of element 18 is based on the Discrete Kirchhoff Quadrilateral (DKQ) [Batoz 1982]. Because the Kirchhoff assumption is enforced, the DKQ is transverse-shear rigid and can only be used for thin shells. No transverse shear stress information is available. The triangle is based on a degeneration of the DKQ. This element sometimes gives slightly lower eigenvalues when compared with element type 20. c) The plate component of element 20 is based on the 8-node serendipity el- ement. At the mid-side, the parallel rotations and transverse displace- ments are constrained and the normal rotations are condensed to yield a 4-node element. The element is based on thick plate theory and is recom- mended for thick and thin plates. d) The quadrilateral elements contain a warpage correction using rigid links. e) The membrane component of element 18 has a zero energy mode associat- ed with in-plane rotations. This is automatically suppressed in a non-flat shell by the plate stiffness of the adjacent elements. In contrast, element 20 has no spurious zero energy modes. 3. Linear Shear Element (22). The linear shear panel element resist tangential in plane shearing along the four edges and can only be used with the elastic mate- rial constants of *MAT_ELASTIC. Membrane forces and out-of-plane loads are not resisted. 4. Simplified Element for Time Domain Vibrations (99). Element type 99 is intended for vibration studies carried out in the time domain. These models may have very large numbers of elements and may be run for relatively long durations. The purpose of this element is to achieve substantial CPU savings. This is achieved by imposing strict limitations on the range of applicability, thereby simplifying the calculations: a) Elements must be rectangular; all edges must parallel to the global 𝑥-, 𝑦- or 𝑧-axis; b) Small displacement, small strain, negligible rigid body rotation; *SECTION_SHELL If these conditions are satisfied, the performance of the element is similar to the fully integrated shell (ELFORM = 16) but at less CPU cost than the default Be- lytschko-Tsay shell element (ELFORM = 2). Single element torsion and in-plane bending modes are included; meshing guidelines are the same as for fully inte- grated shell elements. No damping is included in the element formulation (e.g. volumetric damping). It is strongly recommended that damping be applied, e.g. *DAMPING_PART_- MASS or *DAMPING_FREQUENCY_RANGE. 5. 2D Formulations. For 2D formulations (12-15, 46, 47), nodes must lie in the global 𝑥-𝑦 plane, i.e., the 𝑧-coordinate must be zero. Furthermore, the element normal should be in positive 𝑧 direction. For axisymmetric element formula- tions, the global 𝑦-axis is taken as the axis of symmetry and all nodes must have 𝑥-coordinate values greater than or equal to 0. Shell thickness values on Card 2 are ignored by formulations 13, 14, and 15. For formulation 14 Input values of loads, lumped masses, discrete element stiffnesses, etc. in axisymmetric models are interpreted as values per unit cir- cumference (i.e., per unit length in the circumferential direction) whereas for formulation 15 they are interpreted per radian. Output of forces for shell for- mulation 15 are in units of force per radian, e.g, as in bndout, nodfor, secforc, spcforc, rcforc. The units of forces output for shell formulation 14 are, at pre- sent, inconsistent. For defining contact in 2D simulations, see the entry for the *CONTACT_2D keyword. 6. Shells with Thickness Stretch. Shell element formulation 25 and 26 are the fully integrated shell element based on the Belytschko-Tsay element but with two additional degrees of freedom allowing for a linear variation of strain through the thickness. By default, the thickness field is continuous across the element edges implying that there can be no complex intersections since this would lock up the structure. It assumes a relatively flat surface and is intended primarily for sheets in metal forming. By specifying IDOF = 2, the thickness field is decoupled between elements which makes the element suited for crash. If there are any thickness stretch triangles (formulation 27), IDOF must be set to 2. 7. Seatbelts. Users must input a set of nodes along one of the transverse edges of a seatbelt. If there is no retractor associated with a belt, the node set can be on either edge. If the retractor exists, the edge should be on the retractor side and input in the same sequence of retractor node set. Therefore, another restriction on the seatbelt usage is each belt has its own section definition and a different part. 8. Fracture. XFEM 2D and shell formulations are recommended for brittle or semi-brittle fracture with pre-cracks, see *BOUNDARY_PRECRACK, or geome- try imperfection such as a notch or a hole. XFEM shell formulation can be used for ductile fracture analysis with regularized effective plastic strain criterion. 9. Discrete Kirchoff Theory Shell (17). Shell element formulation 17 (DKT) is based on discrete Kirchhoff theory. It neglects out-of-plane shear strain energy and is thus valid only for thin plates where shear strain energy is negligible compared to bending energy. 10. Limitations of Area-Weight Shell (14). The exact stiffness matrix for the area- weighted shell formulation type 14 is nonsymmetric. The nonsymmetric terms are dropped for computational efficiency, making this formulation unsuitable for implicit linear analysis and eigenvalue analysis. It may, however, be used effectively for implicit nonlinear analysis. For explicit dynamics, viscous hourglass limits high frequency noise that may otherwise lead to nonphysical element distortion when nodes are on or near the axis of symmetry. Viscosity can be added to type 6 or 7 hourglass control by using VDC > 0 under the *HOURGLASS keyword. Alternatively, type 1 hour- glass control is viscous. 11. Eight Node Singular Shell (55). The eight-noded singular element for fracture analysis is based on the eight-noded quadratic quadrilateral element. There are two ways to include the singularity around the crack tip: a) Move the two mid-nodes on the edges connected to the crack tip to the quarter location and obtain a strain singularity of 1/√𝑟 b) Collapse the three nodes on one side of a quadrilateral element to the crack tip (but the three nodes remain independent) and move the two neighboring mid-nodes to the quarter location to obtain a strain singulari- ty of 1/𝑟. This element uses 3×3 quadrature and is available to both implicit and explicit analyses. Cohesive Shell (29). Element type +/-29 is a cohesive element that models cohesive interfaces between shell element edges. The element takes bending forces into account and uses drilling force stabilization. Consider two shell elements in the same plane with nodes 𝑚1, 𝑚2, 𝑚3, 𝑚4, 𝑛1, 𝑛2, 𝑛3, and 𝑛4 such that the (𝑚3, 𝑚4) edge and the (𝑛1, 𝑛2) edge are connected through a cohesive shell having nodes 𝑚4, 𝑚3, 𝑛2, and 𝑛1, see Figure 36-23. The initial area of the cohesive element may be zero, in which case density is de- fined in terms of the length of the single connecting edge. Element type +/-29 works similarly to solid element type 20. For example, extruding the two non-cohesive shells in their respective normal directions defines two 8 node solids. The cohesive mid-surface is located between the opposing faces of the solids, and tractions are calculated in four mid-surface points using differences of displacements between the opposing faces, giving rise to nodal forces and moments in the cohesive shell nodes 𝑚4, 𝑚3, 𝑛2, and 𝑛1. Additional details can be found in the Theory Manual. Difference between type 29 and -29: In both formulations, the cohesive coordi- nate system direction 𝑞2 is defined by the midpoints of the (𝑛1, 𝑚4) and (𝑛2, 𝑚3) edges. Type 29 defines the cohesive midsurface normal 𝑞3 using the midpoints on the far side edges (𝑚1, 𝑚2) and (𝑛3, 𝑛4), while type -29 defines 𝑞1 to be the mean of the neighboring element normals. Thus, in pure out-of-plane shear, type 29 will initially have pure tangential traction that turns into a normal trac- tion as the separation increases, while type -29 will only have tangential trac- tion. 𝒒3 𝑛4 𝑛1 𝑚4 𝑚1 𝒒1 𝑛3 𝑛2 𝑚3 𝑚2 𝒒2 Figure [36-23]. Cohesive interface coordinate system for element type +/-29 12. Accurate fully-integrated shell (-16). Accuracy issues have been observed in shell formulation 16 under large deformations/rotations over a single time step. Formulation -16 is a correspondently enhanced version of formulation 16. Formulation 16 is unchanged to maintain back compatibility and, although, element -16 is supported in explicit mode it is primarily intended for implicit time integration. A strongly objective version can be activated by combining ELFORM = -16 and IACC = 1 on *CONTROL_ACCURACY, thereby ensuring that arbitrarily large rigid body rotation in a single step will transform stresses correctly and not generate any spurious strains. 13. XFEM ductile fracture. This feature is supported by a joint research among Honda, JSOL and LSTC. For FAILCR = -2, the failure strain is defined by: EPS = FS+(FS1-FS)*min(L/CL, 1.0) where L is the current crack length. Example: $$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ $ $$$$ *SECTION_SHELL $ $$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ $ $ Define a shell section that specifies the following: $ elform = 10 Belytschko-Wong-Chiang shell element formulation. $ nip = 3 Three through the shell thickness integration points. $ t1 - t4 = 2.0 A shell thickness of 2 mm at all nodes. $ *SECTION_SHELL $ $...>....1....>....2....>....3....>....4....>....5....>....6....>....7....>....8 $ sid elform shrf nip propt qr/irid icomp 1 10 3.0000 $ $ t1 t2 t3 t4 nloc 2.0 2.0 2.0 2.0 $ $$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ *SECTION_SOLID_{OPTION} Available options include: <BLANK> EFG SPG Purpose: Define section properties for solid continuum and fluid elements. Card Sets. For each unique solid section, include one set of data cards. The EFG option and the SPG option cannot both appear in the same model. This input ends at the next keyword (“*”) card. Card 1 1 2 3 4 5 6 7 8 Variable SECID ELFORM AET Type I/A I I EFG Card. Additional card for the EFG keyword option. See *CONTROL_EFG. 3 4 5 6 7 8 DZ ISPLINE IDILA IEBT IDIM TOLDEF Card 2 Variable 1 DX Type F 2 DY F Default 1.01 1.01 1.01 F I 0 I 0 I 1 I 2 F 0.01 Optional EFG Card. Additional optional card for the EFG keyword option. See *CON- TROL_EFG. Card 3 1 2 3 Variable IPS STIME IKEN Type Default I 0 F 1020 I 0 4 SF I 0.0 5 6 CMID IBR I I 1 7 DS F 8 ECUT F 1.01 0.1 SPG Card. Additional card for the SPG keyword option. 3 4 5 6 7 8 DZ ISPLINE KERNEL LSCALE SMSTEP SWTIME Card 2 Variable 1 DX Type F 2 DY F Default 1.50 1.50 1.50 F I 0 I 0 F I F 15 Optional SPG Card. Additional optional card for the SPG keyword option. Card 3 1 2 3 4 5 6 7 8 Variable IDAM FS STRETCH ITB Type Default I 0 F F I User Defined Element Card. Additional card for ELFORM = 101, 102, 103, 104 or 105. See Appendix C. Card 1 2 3 4 5 6 7 8 Variable NIP NXDOF IHGF ITAJ LMC NHSV Type Default I 0 I 0 I 0 I 0 I 0 I 0 Integration Point Card. Additional card for ELFORM = 101, 102, 103, 104 or 105. Add NIP cards adhering to the format below. Because the default value for NIP is 0, these cards are read only for user-defined elements. See Appendix C. Card Variable Type 1 XI F 2 3 4 5 6 7 8 ETA ZETA WGT F F F Default none none none none Property Parameter Cards. Additional card for ELFORM = 101, 102, 103, 104 or 105. Add LMC property parameters by packing 8 parameters per card. See Appendix C. Card Variable Type Default 1 P1 F 0 2 P2 F 0 3 P3 F 0 4 P4 F 0 5 P5 F 0 6 P6 F 0 7 P7 F 0 8 P8 F 0 VARIABLE SECID DESCRIPTION Section ID. SECID is referenced on the *PART card. A unique number or label must be specified. ELFORM Element formulation options. Remark 2 enumerates the element VARIABLE DESCRIPTION formulations available for implicit calculations: EQ.-2: EQ.-1: EQ.0: EQ.1: EQ.2: EQ.3: EQ.4: EQ.5: EQ.6: EQ.7: EQ.8: EQ.9: EQ.10: EQ.11: EQ.12: EQ.13: Fully integrated S/R solid intended for elements with poor aspect ratio, accurate formulation Fully integrated S/R solid intended for elements with poor aspect ratio, efficient formulation 1 point corotational for *MAT_MODIFIED_HONEY- COMB Constant stress solid element: default element type. By specifying hourglass type 10 with this element, a Cosserat Point Element is invoked, see *CON- TROL_HOURGLASS Fully integrated S/R solid Fully integrated quadratic 8 node element with nodal rotations S/R quadratic tetrahedron element with nodal rotations 1 point ALE 1 point Eulerian 1 point Eulerian ambient Acoustic 1 point corotational for *MAT_MODIFIED_HONEY- COMB 1 point tetrahedron 1 point ALE multi-material element 1 point integration with single material and void 1 point nodal pressure tetrahedron EQ.14: 8 point acoustic EQ.15: EQ.16: 2 point pentahedron element 4 or 5 point 10-noded tetrahedron . By specifying hourglass type 10 with this element, a Cosserat Point Element is invoked, see *CONTROL_- HOURGLASS VARIABLE DESCRIPTION EQ.17: EQ.18: EQ.19: EQ.20: EQ.21: EQ.22: 10-noded composite tetrahedron 8 point enhanced strain solid element for linear statics only 8-noded, 4 point cohesive element 8-noded, 4 point cohesive element with offsets for use with shells 6-noded, 1 point pentahedron cohesive element 6-noded, 1 point pentahedron cohesive element with offsets for use with shells EQ.23: 20-node solid formulation EQ.24: 27-noded, fully element integrated S/R quadratic solid EQ.41: Mesh-free (EFG) solid formulation EQ.42: Adaptive 4-noded mesh-free (EFG) solid formulation EQ.43: Mesh-free enriched finite element EQ.45: Tied Mesh-free enriched finite element EQ.47: Smoothed particle Galerkin method EQ.98: Interpolation solid EQ.99: Simplified linear element for time-domain vibration studies EQ.101: User defined solid EQ.102: User defined solid EQ.103: User defined solid EQ.104: User defined solid EQ.105: User defined solid EQ.115: 1 point pentahedron element with hourglass control GE.201: Isogeometric solids with NURBS. GE.1000: Generalized user-defined solid element formulation VARIABLE DESCRIPTION AET Ambient Element type: Can be defined for ELFORM 7, 11 and 12. EQ.0: Non-ambient EQ.1: Temperature (not currently available) EQ.2: Pressure and temperature (not currently available) EQ.3: Pressure outflow (obsolete) EQ.4: Pressure inflow/outflow (Default for ELFORM 7) EQ.5: Receptor for blast load Normalized dilation parameters of the kernel function in 𝑥, 𝑦 and 𝑧 directions. The normalized dilation parameters of the kernel function are introduced to provide the smoothness and compact support properties on the construction of the mesh-free shape functions. Values between 1.0 and 1.5 are recommended. Values smaller than 1.0 are not allowed. Larger values will increase the computation time and will sometimes result in a divergence problem. DX, DY, DZ ISPLINE Replace the choice for the EFG kernel functions definition in *CONTROL_EFG. This allows users to define different ISPLINE in different sections. EQ.0: Cubic spline function (default). EQ.1: Quadratic spline function. EQ.2: Cubic spline function with circular shape. IDILA Replace the choice for the normalized dilation parameter definition in *CONTROL_EFG. This allows users to define different IDILA in different sections. EQ.0: Maximum distance based on the background elements. EQ.1: Maximum distance based on surrounding nodes. IEBT Essential boundary condition treatment: See Remark 9 and 10. EQ.1: Full transformation method (default) EQ.-1: (w/o transformation) EQ.2: Mixed transformation method EQ.3: Coupled FEM/EFG method VARIABLE DESCRIPTION EQ.4: Fast transformation method EQ.-4: (w/o transformation) EQ.5: Fluid particle method for E.O.S and *MAT_ELASTIC_- FLUID materials, currently supports only 4-noded background elements. EQ.7: Maximum entropy approximation IDIM Domain integration method: See Remark 11. EQ.1: Local boundary integration EQ.2: Two-point Gauss integration (default) EQ.3: Improved Gauss integration for IEBT = 4 or -4 EQ.-1: Stabilized EFG integration method (apply to 6-noded cell, 8-noded cell or combination of these two) EQ.-2: EFG fracture method (apply to 4-noded cell and SMP only) TOLDEF Deformation tolerance for the activation of adaptive EFG Semi- Lagrangian and Eulerian kernel. See Remark 12. EQ.0.0: Lagrangian kernel GT.0.0: Semi_Lagrangian kernel LT.0.0: Eulerian kernel IPS EQ.0: No pressure smoothing (default) EQ.1: Moving-least squared pressure recovery STIME Time to switch from stabilized EFG to standard EFG formulation IKEN EQ.0: Moving-least-square approximation (default, recom- mended) EQ.1: Maximum Entropy approximation SF CMID Failure strain, recommended as an extra condition for the crack initiation under slow loading besides the stress-based cohesive law Cohesive material ID for EFG fracture analysis (only Mode I crack is considered and only *MAT_COHESIVE_TH is available) VARIABLE DESCRIPTION IBR DS ECUT EQ.1: No branching allowed EQ.2: Branching is allowed Normalized support defined for computing the displacement jump in fracture analysis Define the minimum distance to the node that a crack surface can cut to the edge KERNEL Type of kernel approximation EQ.0: updated Lagrangian kernel, no failure, less shear deformation EQ.1: Eulerian kernel, deformation failure analysis, global extreme EQ.2: Semi-pseudo Lagrangian kernel, failure analysis, local extreme deformation LSCALE Length scale for displacement regularization (not used yet) SMSTEP Interval of time steps to conduct displacement regularization SWTIME Time to switch from updated Lagrangian kernel to Eulerian kernel IDAM Option of damage mechanism EQ.0: Continuum damage mechanics (default), the failed nodes are not eroded but converted to free nodes still carrying mass and momentum EQ.1: Phenomenological strain damage FS Failure effective plastic strain if IDAM = 1 STRETCH Stretching parameter if IDAM = 1 ITB Flag for using stabilization EQ.0: standard meshfree approximation + T-bond algorithm EQ.1: fluid particle approximation (accurate but slow) EQ.2: simplified fluid particle approximation (efficient and robust) failure NIP *SECTION_SOLID DESCRIPTION Number of integration points for user-defined solid (0 if resultant element) NXDOF Number of extra degrees of freedom per node for user-defined solid IHGF Flag for using hourglass stabilization (NIP.GT.0) EQ.0: Hourglass stabilization is not used EQ.1: LS-DYNA hourglass stabilization is used EQ.2: User-defined hourglass stabilization is used EQ.3: Same as 2, but the resultant material tangent moduli are passed ITAJ Flag for setting up finite element matrices (NIP.GT.0) EQ.0: Set up matrices wrt isoparametric domain EQ.1: Set up matrices wrt physical domain LMC Number of property parameters NHSV Number of history variables XI ETA ZETA WGT First isoparametric coordinate Second isoparametric coordinate Third isoparametric coordinate Isoparametric weight PI Ith property parameter Remarks: 1. ESORT to Stabilize Degenerate Solids. The ESORT variable of the *CON- TROL_SOLID keyword can be set to automatically convert degenerate tetrahe- into more suitable solid element drons and degenerate pentahedrons formulations. The sorting is performed internally and is transparent to the user. See *CONTROL_SOLID for details. 2. Implicit Analysis. For implicit calculations the following element choices are implemented: EQ.-2: Fully integrated S/R solid element for poor aspect ratios, ac- curate formulation. EQ.-1: Fully integrated S/R solid element for poor aspect ratios, effi- cient formulation. EQ.1: Constant stress solid element. EQ.2: Fully integrated S/R solid. EQ.3: Fully integrated 8 node solid with rotational DOFs. EQ.4: Fully integrated S/R 4 node tetrahedron with rotational DOFs. EQ.10: 1 point tetrahedron. EQ.13: 1 point nodal pressure tetrahedron. EQ.15: 2 point pentahedron element. EQ.16: 5 point 10-noded tetrahedron. EQ.17: 10-noded composite tetrahedron. EQ.18: 8 point enhanced strain solid element for linear statics only. EQ.19: 8-noded, 4 point cohesive element EQ.20: 8-noded, 4 point cohesive element with offsets for use with shells EQ.21: 6-noded, 1 point pentahedron cohesive element EQ.22: 6-noded, 1 point pentahedron cohesive element with offsets for use with shells EQ.23: 20-node solid formulation EQ.24: 27-node solid formulation EQ.41: Mesh-free (EFG) solid formulation. EQ.42: 4-noded mesh-free (EFG) solid formulation. EQ.43: Mesh-free enriched finite element. If another element formulation is requested, LS-DYNA will substitute, when possible, one of the above in place of the one chosen. The type 1 element, con- stant stress, is generally much more accurate than the type 2 element, the selec- tive reduced integrated element for implicit problems. 3. Element for Modified Honeycomb Material. Element formulations 0 and 9, applicable only to *MAT_MODIFIED_HONEYCOMB, behave essentially as nonlinear springs so as to permit severe distortions sometimes seen in honey- comb materials. In formulation 0, the local coordinate system follows the ele- ment rotation whereas in formulation 9, the local coordinate system is based on axes passing through the centroids of the element faces. Formulation 0 is pre- ferred for severe shear deformation where the barrier is fixed in space. If the barrier is attached to a moving body, which can rotate, then formulation 9 is usually preferred. 4. Elements for Shear and Pressure Locking: Types 2 and 18. The selective reduced integrated solid element, element type 2, assumes that pressure is constant throughout the element to avoid pressure locking during nearly in- compressible flow. However, if the element aspect ratios are poor, shear lock- ing will lead to an excessively stiff response. A better choice, given poor aspect ratios, is the one point solid element which work well for implicit and explicit calculations. For linear statics, the type 18 enhanced strain element works well with poor aspect ratios. Please note that highly distorted elements should always be avoided since excessive stiffness will still be observed even in the enhanced strain formulations. 5. Element Type 99 for Vibration. Element type 99 is intended for vibration studies carried out in the time domain. These models may have very large numbers of elements and may be run for relatively long durations. The pur- pose of this element is to achieve substantial CPU savings. This is achieved by imposing strict limitations on the range of applicability, thereby simplifying the calculations: a) Elements must be cubed; all edges must parallel to the global 𝑥-, 𝑦- or 𝑧- axis; b) Small displacement, small strain, negligible rigid body rotation; c) Elastic material only If these conditions are satisfied, the performance of the element is similar to the fully integrated S/R solid (ELFORM = 2) but at less CPU cost than the default solid element (ELFORM = 1). Single element bending and torsion modes are included, so meshing guidelines are the same as for fully integrated solids – e.g. relatively thin structures can be modeled with a single solid element through the thickness if required. Typically, the CPU requirement per element-cycle is roughly two thirds that of the default solid element. No damping is included in the element formulation (e.g. volumetric damping). It is strongly recommended that damping be applied, e.g. *DAMPING_PART_- MASS or *DAMPING_FREQUENCY_RANGE. Δx84 Δx51 Δx62 Midsurface Δx73 Figure 36-24. Illustration of solid local coordinates. 6. 8-Node Cohesive Element: Type 19. Element type 19 is a cohesive element. The tractions on the mid-surface defined as the mid-points between the nodal pairs 1-5, 2-6, 3-7, and 4-8 are functions of the differences of the displacements between nodal pairs interpolated to the four integration points. The initial volume of the cohesive element may be zero, in which case, the density may be defined in terms of the area of nodes 1-2-3-4. See Appendix A and the user material description for additional details. See also *MAT_ADD_COHESIVE. The tractions are calculated in the local coordinate system defined at the cen- troid of the element, see the Figure 36-24. Defining the rotation matrix from the local to the global coordinate system at time 𝑡 as 𝐑(𝑡), the initial coordinates as 𝐗, and the current coordinates as x, the displacements at an integration point are Δ𝐮 = 𝐑T(𝑡)Δ𝐱 − 𝐑T(0)Δ𝐗 Δ𝐱 = ∑ 𝑁𝑖(𝑠, 𝑡)Δ𝐱𝑖+4,𝑖 𝑖=1 Δ𝐗 = ∑ 𝑁𝑖(𝑠, 𝑡)Δ𝐗𝑖+4,𝑖 𝑖=1 The forces are obtained by integrating the tractions over the mid-surface, and rotating them into the global coordinate system. It is the sum over integration points g = 1,2,3,4. 𝐅𝑖 = 𝐑(𝑡) ∑ 𝐓𝑔𝑁𝑖(𝑠𝑔, 𝑡𝑔) det(J𝑔) , for 1 ≤ 𝑖 ≤ 4, and 𝐅𝑖+4 = −𝐅𝑖 𝑔=1 Where, 𝐓𝑔 = is the traction stress in the local coordinate system 𝑁𝑖 = The shape function of the cohesive element at node i 𝑠𝑔 and 𝑡𝑔 = The parameteric coordinates of the 4 integration points Jg = The integration point’s portion of the determinate of the cohesive element which is equivalent to the element volume 7. 6-Node Cohesive Element: Type 21. Element type 21 is the pentahedral counterpart to element type 19 with three nodes on the bottom and top surface. The tractions on the mid-surface are defined as the mid-points between the nodal pairs 1-5, 2-6, and 3-7 are functions of the differences of the displace- ments between nodal pairs interpolated to one integration point. The ordering of the nodal points in *ELEMENT_SOLID is given by: 6-noded (cohesive) pentahedron N1, N2, N3, N3, N5, N6, N7, N7, 0, 0 Setting ESORT.gt.0 in *CONTROL_SOLID will automatically sort degenerated cohesive elements type 19 to cohesive pentahedron elements type 21. 8. Cohesive Element with Offsets: Types 20 and 22. Element type 20 is identical to element 19 but with offsets for use with shells. The element is as- sumed to be centered between two layers of shells on the cohesive element’s lower (1-2-3-4) and upper (5-6-7-8) surfaces. The offset distances for both shells are one half the initial thicknesses of the nodal pairs (1-5, 2-6, 3-7, and 4-8) sepa- rating the two shells. These offsets are used with the nodal forces to calculate moments that are applied to the shells. Element type 20 in tied contacts will work correctly with the option, TIED_SHELL_EDGE_TO_SURFACE, which transmits moments. Other tied options will leave the rotational degrees-of- freedom unconstrained with the possibility that the rotational kinetic energy will cause a large growth in the energy ratio. Element type 22 is the pentahedron counterpart to element type 20 with three nodes on the bottom and top surface. The ordering of the nodal points in *ELE- MENT_SOLID are identical to element type 21 . Setting ES- ORT.GT.0 in *CONTROL_SOLID will automatically sort degenerated cohesive elements type 20 to cohesive pentahedron elements type 22. 9. Automatic Sorting for EFG Background Mesh. The current EFG formulation performs automatic sorting for finite element tetrahedral, pentahedron, and hexahedral elements as the background mesh to identify the mesh-free geome- try and provide the contact surface definition in the computation. 10. Essential Boundary Conditions. The mixed transformation method, the coupled FEM/EFG method and the fast transformation method were imple- mented in EFG 3D solid formulation. These three features were added to im- prove the efficiency on the imposition of essential boundary conditions and the transfer of real nodal values and generalized nodal values. The mixed trans- formation method is equivalent to the full transformation method with im- proved efficiency. The behavior of the coupled FEM/EFG method is between FEM and EFG. The fast transformation method provides the most efficient and robust results. 11. IDIM. For compressible material like foam and soil, IDIM=1 is recommended. For nearly incompressible material like metal and rubber, IDIM=2 (default) is recommended. 12. TOLDEF. This parameter is introduced to improve the negative volume problem usually seen during large deformation analysis. For the same analysis, the larger value of Toldef, the earlier Semi-Lagrangian or Eulerian kernel is introduced into the EFG computation and more cpu time is expected. Value between 0.0 and 0.1 is suggested in the crashworthiness analysis. Semi- Lagrangian kernel is suggested for the solid materials and Eulerian kernel is suggested for the fluid and E.O.S. materials. 13. 10-Node Tetrahedra: Types 16 and 17. Formulations 16 and 17 are 10-noded, tetrahedral formulations. The parameter NIPTETS in *CONTROL_SOLID controls the number of integration points for these formulations. Formulation 17 is generally preferred over formulation 16 because, unlike 16, the nodal weighting factors are equal and thus nodal forces from contact and applied pressures are distributed correctly. When applying loads to 10-noded tetrahedrons via segments, no load will be applied to the midside nodes if the segments contain only corner nodes. When defining contact, it is recommended that *CONTACT_AUTOMATIC_… be used and the contact surface of the 10-noded tetrahedral part be specified by its part ID. In this manner, midside nodes receive contact forces. If the 10-noded element connectivity is not defined in accordance with the fig- ure shown in *ELEMENT_SOLID, the order of the nodes can be quickly changed via a permutation vector specified with *CONTROL_SOLID. If *ELE- MENT_SOLID defines 4-noded tetrahedrons, you can easily convert to 10- noded tetrahedrons using the command *ELEMENT_SOLID_TET4TOTET10. Because the characteristic length of a 10-noded tetrahedron is half that of a 4- noded tetrahedron, the time step for the tetrahedrons will be smaller by a factor of 2. The parameter TET10 in 971, when set to 1 in *CONTROL_OUTPUT, causes the full 10-node connectivity to be written to the d3plot and d3part data- bases. 14. 1-Point Nodal Pressure Tetrahedron: Type 13. Element type 13 is identical with type 10 but with additional averaging of nodal pressures, which signifi- cantly lowers volumetric locking. Therefore, it is well suited for applications with incompressible and nearly incompressible material behavior, i.e. rubber materials or ductile metals with isochoric plastic deformations (e.g. bulk form- ing). Compared to the standard tetrahedron (type 10), a speed penalty of max. 25 % can be observed. In implicit, all material models supported by type 10 are also supported for this element, while for explicit currently material models *MAT_001, 003, 006, 007, 015, 024, 027, 077, 081, 082, 091, 092, 098, 103, 106, 120, 123, 124, 128, 129, 181, 183, 187, 224, 225, and 244 are fully supported. For other materials this element behaves like the type 10 tetrahedron. 15. Fully Integrated S/R Solid Elements for Elements with Poor Aspect Ratio: Types -1 and -2. Solid formulations -1 and -2 may offer improved behavior over formulation 2 by accounting for poor element aspect ratios in a manner so as to reduce the transverse shear locking effects seen in formulation 2. Type -1 is a more computationally efficient implementation of type -2, but a side-effect is that type -1’s resistance to a particular deformation mode, similar to an hour- glass mode, is weakened. This side effect is not truly hourglassing behavior and so there is no hourglass energy and behavior is not affected by hourglass parameters. 16. EFG Solid Elements: Types 41 and 42. EFG element type 41 supports 4-node, 6-node and 8-node solid elements. For 3D tetrahedron 𝑟-adaptive analysis (AD- POPT=7 in *CONTROL_ADAPTIVE and ADPOPT=2 in *PART), if the initial mesh is not purely comprised of tetrahedrons, element type 41 should be used instead of 42 causing the mesh to be converted automatically into tetrahedron after the first time step. Element type 42 only supports 4-node tetrahedron mesh, and is optimized to achieve better computational efficiency compared to 41. 17. Smoothed Particle Galerkin (SPG) method: Type 47. In SPG method, nodes are converted into particles and 4-node, 6-node and 8-node solid elements are supported. The method is suitable for severe deformation problem and failure analysis. *SECTION (Note: NODE_SET option is available starting with the R3 release of Version 971) $$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ $ $$$$ *SECTION_SOLID $ $$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ $ $ A bolt modeled with solids was found to have excessive hourglassing. $ Thus, the section (sid = 116) associated with the bolt part was used $ to specify that a fully integrated Selectively-Reduced solid element $ formulation be used to totally eliminate the hourglassing (elform = 2). $ *SECTION_SOLID $...>....1....>....2....>....3....>....4....>....5....>....6....>....7....>....8 $ sid elform 116 2 $ *PART bolts $ pid sid mid eosid hgid adpopt 17 116 5 $ $$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ *SECTION_SPH_{OPTION} Available options include: <BLANK> ELLIPSE INTERACTION USER Purpose: Define section properties for SPH particles. NOTE: This feature is not supported for use in implicit cal- culations. Card Sets. For each SPH section add one set of cards 1 or 2 (depending on the keyword option). This input ends at the next keyword (“*”) card. Card 1 1 2 3 4 5 6 7 8 Variable SECID CSLH HMIN HMAX SPHINI DEATH START Type I/A F F F F F F Default none 1.2 0.2 2.0 0.0 1.e20 0.0 Ellipse Card. Additional card for ELLIPSE keyword option. Card 2 1 2 3 4 5 6 7 8 Variable HXCSLH HYCSLH HZCSLH HXINI HYINI HZINI Type F F F F F F VARIABLE SECID DESCRIPTION Section ID. SECID is referenced on the *PART card. A unique number or label must be specified. CSLH *SECTION DESCRIPTION Constant applied to the smoothing length of the particles. The default value applies for most problems. Values between 1.05 and 1.3 are acceptable. Taking a value less than 1 is inadmissible. Values larger than 1.3 will increase the computational time. The default value is recommended. HMIN Scale factor for the minimum smoothing length HMAX Scale factor for the maximum smoothing length SPHINI Optional initial smoothing length (overrides true smoothing length). This option applies to avoid LS-DYNA to calculate the smoothing length during initialization. In this case, the variable CSLH doesn't apply. DEATH Time imposed SPH approximation is stopped. START Time imposed SPH approximation is activated. Constant applied for the smoothing length in the 𝑥-direction for the ellipse case. Constant applied for the smoothing length in the 𝑦-direction for the ellipse case. Constant applied for the smoothing length in the 𝑧-direction for the ellipse case. Optional initial smoothing length in the 𝑥-direction for the ellipse case (overrides true smoothing length) Optional initial smoothing length in the 𝑦-direction for the ellipse case (overrides true smoothing length) Optional initial smoothing length in the 𝑧-direction for the ellipse case (overrides true smoothing length) HXCSLH HYCSLH HZCSLH HXINI HYINI HZINI Remarks: 1. Smoothing Length. The SPH processor in LS-DYNA employs a variable smoothing length. LS-DYNA computes the initial smoothing length, ℎ0, for each SPH part by taking the maximum of the minimum distance between every particle. Every particle has its own smoothing length which varies in time according to the following equation: 𝑑𝑡 ℎ(𝑡) = ℎ(𝑡)∇ ⋅ v where ℎ(𝑡) is the smoothing length, and where ∇ ⋅ 𝐯 is the divergence of the flow. The smoothing length increases as particles separate and reduces as the concentration increases. This scheme is designed to hold constant the number of particles in each neighborhood. In addition to being governed by the above evolution equation the smoothing length is constrained to be between a user- defined upper and lower value HMIN × ℎ0 < ℎ(𝑡) < HMAX × ℎ0. Defining a value of 1 for HMIN and 1 for HMAX will result in a constant smoothing length in time and space. 2. USER Option. The USER option allows the definition of customized subrou- tine for the variation of the smoothing length. A subroutine called hdot is de- fined in the file dyn21.F (Unix/linux) or lsdyna.f (Windows). 3. Contact/Partial Interaction. Combined with CONT=1 the *CONTROL_SPH card, this keyword option activates a partial interaction be- tween SPH parts through the normal interpolation method and partially inter- act through the contact option. All the SPH parts defined using this keyword will interact with each other through normal interpolation method automatical- ly. in *SECTION Purpose: Define section properties for thick shell elements. Card Sets. For each TSHELL section include a set of the following cards. This input ends at the next keyword (“*”) card. Card 1 1 2 3 4 5 6 7 8 Variable SECID ELFORM SHRF NIP PROPT QR ICOMP TSHEAR Type I/A Default none I 1 F 1.0 F 2 F 1 F 0 I 0 I 0 Angle Cards. If ICOMP = 1 specify NIP angles putting 8 on each card. Include as many cards as necessary. Card 2 Variable 1 B1 Type F 2 B2 F 3 B3 F 4 B4 F 5 B5 F 6 B6 F 7 B7 F 8 B8 F VARIABLE SECID DESCRIPTION Section ID. SECID is referenced on the *PART card. A unique number or label must be specified. ELFORM Element formulation: EQ.1: one point reduced integration (default), EQ.2: selective reduced 2 × 2 in plane integration. EQ.3: assumed strain 2 × 2 in plane integration, see remark below. EQ.5: assumed strain reduced integration with brick materials EQ.6: assumed strain reduced integration with shell materials EQ.7: assumed strain 2 × 2 in plane integration. SHRF Shear factor. A value of 5/6 is recommended . NIP *SECTION_TSHELL DESCRIPTION Number of through thickness integration points for the thick shell. See the variable INTGRD in *CONTROL_SHELL for details of the through thickness integration rule. EQ.0: set to 2 integration points. PROPT Printout option: EQ.1.0: average resultants and fiber lengths, EQ.2.0: resultants at plan points and fiber lengths, EQ.3.0: resultants, stresses at all points, fiber lengths. QR Quadrature rule: LT.0.0: absolute value is specified rule number, EQ.0.0: Gauss (up to five points are permitted), EQ.1.0: trapezoidal, not recommended for accuracy reasons. ICOMP Flag for layered composite material mode: EQ.1: a material angle is defined for each through thickness integration point. For each layer one integration point is used. TSHEAR Flag for transverse shear strain or stress distribution : EQ.0.0: Parabolic, EQ.1.0: Constant through thickness. B1 B2 B3 ⋮ 𝛽1, material angle at first integration point. The same procedure for determining material directions is use for thick shells that is used for the 4 node quadrilateral shell. 𝛽2, material angle at second integration point 𝛽3, material angle at third integration point ⋮ BNIP 𝛽NIP, material angle at eighth integration point *SECTION 1. Thick Shell Element Formulations. Thick shell elements are bending elements that have 4 nodes on the bottom face and 4 on the top face. Thick shell element formulations 1, 2 and 6 are extruded thin shell elements and use thin shell material models and have an uncoupled stiffness in the z-direction. Thick shell element formulations 3, 5, and 7 are layered brick elements that use 3D brick material models. Element forms 3 and 5, and 6 are distortion sensitive and should not be used in situations where the elements are badly shaped. A single thick shell element through the thickness will capture bending response, but with element types 3, at least two are recommended to avoid excessive softness. 2. Formulation 1 Quadrature Quirk. When using Gauss quadrature with element formulation 1 the number of integration point is automatically switched to 3 when NIP = 2 and 5 when NIP = 4. 3. Implicit Time Integration. Thick shell elements are available for implicit analysis with the exception of thick shell formulation 1. If an element of type 1 is specified in an implicit analysis, it is internally switched to type 2 4. SHRF Field. For ELFORM=1, 2 and 6, the transverse shear stiffness is scaled by the SHRF parameter. Since the strain is assumed to be constant through the thickness, setting SHRF=5/6 is recommended to obtain the correct shear ener- gy. For ELFORM=3 and 5, the SHRF parameter is not used, except for material types 33, 36, 133, 135, and 243. For ELFORM=3, the shear stiffness is assumed constant through the thickness. For ELFORM=5, 6, and 7, the shear distribu- tion is assumed either parabolic if TSHEAR=0, or constant if TSHEAR=1. The parabolic assumption is good when the elements are used in a single layer to model a shell type structure, but the constant option may be better when ele- ments are stacked one on top of the other. 5. Modeling Composites. Thick shell elements of all formulations can be used to model layered composites, but element formulations 5 and 6 use assumed strain to capture the complex Poisson’s effects and through thickness stress distribution in layered composites. To define the layers of a composite, use QR < 0 to point to *INTEGRATION_SHELL data. Alternatively, the *PART_- COMPOSITE_TSHELL keyword offers a simplified way to define the layers. When modeling composites, laminated shell theory may be used to correct the transverse shear strain if the shear stiffness varies by layer. Laminated shell theory is activated by setting LAMSHT = 4 or 5 on *CONTROL_SHELL. When laminated shell theory is active, the TSHEAR parameter works with all ELFORM values to select either a parabolic or constant shear stress distribution. The keyword *SENSOR provides a convenient way of activating and deactivating boundary conditions, airbags, discrete elements, joints, contact, rigid walls, single point constraints, and constrained nodes. The sensor capability is new in the second release of version 971 and will evolve in later releases to encompass many more LS-DYNA capabilities and replace some of the existing capabilities such as the airbag sensor logic. The keyword commands in this section are defined below in alphabetical order: *SENSOR_CONTROL *SENSOR_CPM_AIRBAG *SENSOR_DEFINE_CALC-MATH *SENSOR_DEFINE_ELEMENT *SENSOR_DEFINE_FORCE *SENSOR_DEFINE_FUNCTION *SENSOR_DEFINE_MISC *SENSOR_DEFINE_NODE *SENSOR_SWITCH *SENSOR_SWITCH_CALC-LOGIC *SENSOR_SWITCH_SHELL_TO_VENT To define and utilize a sensor, three categories of sensor keyword commands are needed as shown in Figure 37-1. 1. Sensors are defined using the *SENSOR_DEFINE commands. Sensors provide a time history of model response that may be referred to by *SENSOR_SWITCH as a switching criterion. (Note: The time history of any sensor can be output using the SENSORD function in *DEFINE_CURVE_FUNCTION and *DATA- BASE_CURVOUT.) a) *SENSOR_DEFINE(_ELEMENT,_FORCE,_MISC,_NODE) These commands define a sensor’s ID, type, and location.. b) *SENSOR_DEFINE_CALC-MATH, *SENSOR_DEFINE_FUNCTION *SENSOR_DEFINE SENSORID TYPE $ Perform math computation on sensor results *SENSOR_DEFINE_CALC-MATH SENSORID MATH SENSID1 SENSID2 .. $Define switch criterion *SENSOR_SWITCH SWITCHID TYPE SENSORID LOGIC VAL $Perform logic computation on SWITCH results *SENSOR_SWITCH_CALC-LOGIC SWITCHID SENSID1 SENSID2 ... $Define how and what to switch *SENSOR_CONTROL CONTROL ID TYPE TYPE CNTC_ID INIT_STA SWITCHID1 SWITCHID2 $Entity to be controlled by sensor *CONTACT_......_ID CNTC_ID Figure 37-1. Relationship between sensor keyword definitions. These commands define a sensor whose value is a mathmatical expression involving other sensors’ values. 2. Sensor switching criterion definition using the *SENSOR_SWITCH keyword, which can be combined with the logical calculation command *SENSOR_- SWITCH_CALC-LOGIC for more complicated definitions. The logic value yielded by this category of commands can be referred by *SENSOR_CONTROL to determine if a status switch condition is met. a) *SENSOR_SWITCH This command compares the numerical value from *SENSOR_DEFINE or *SENSOR_DEFINE_CALC-MATH with the given criterion to see if a switching condition is met. b) *SENSOR_SWITCH_CALC-LOGIC This command performs logical calculation on the information from SENSOR_SWITCH. 3. Sensor control definition, *SENSOR_CONTROL. This category of commands determines how and what to switch based on the logical values from *SEN- SOR_SWITCH and/or *SENSOR_SWITCH_CALC-LOGIC. *SENSOR Purpose: This command uses switches (*SENSOR_SWITCH) to toggle on or off the effects of other LS-DYNA keywords such as *CONTACT, or *AIRBAG. Card Sets. For each sensor control add a pair of cards 1 and 2. This input ends at the next keyword (“*”) card. Card 1 1 2 3 4 5 6 7 8 Variable CNTLID TYPE TYPEID TIMEOFF NREP Type I Card 2 1 A 2 I 3 I 4 I 5 6 7 8 Variable INITSTT SWIT1 SWIT2 SWIT3 SWIT4 SWIT5 SWIT6 SWIT7 Type A I I I I I I I VARIABLE DESCRIPTION CNTLID Sensor control ID. TYPE Entity to be controlled: EQ.“AIRBAG”: *AIRBAG EQ.“BAGVENTPOP”: Opening and closing the airbag venting holes EQ.“BELTPRET”: Belt pretensioner firing EQ.“BELTRETRA”: Locking the belt retractor EQ.“BELTSLIP”: Controling the slippage of slip ring element EQ.“CONTACT”: *CONTACT EQ.“CONTACT2D”: *CONTACT_2D EQ.“CPM” *AIRBAG_PARTICLE EQ.“DEF2RIG”: *DEFORMABLE_TO_RIGID_AUTO- MATIC *SENSOR_CONTROL DESCRIPTION EQ.“ELESET”: Element set, see “ESTYP” below. EQ.“FUNCTION”: *DEFINE_CURVE_FUNCTION Remarks 5 & 6) (see EQ.“JOINT”: *CONSTRAINED_JOINT EQ.“JOINTSTIF”: *CONSTRAINED_JOINT_STIFFNESS EQ.“M PRESSURE”: *LOAD_MOVING_PRESSURE EQ.“POREAIR”: *MAT_ADD_PORE_AIR EQ.“PRESC-MOT”: *BOUNDARY_PRESCRIBED_MOTION EQ.“PRESC-ORI”: *BOUNDARY_PRESCRIBED_ORIENTA- TION_RIGID EQ.“PRESSURE”: *LOAD_SEGMENT_SET EQ.“RWALL”: *RIGID_WALL EQ.“SPC”: *BOUNDARY_SPC EQ.“SPOTWELD”: *CONSTRAINED_SPOTWELD TYPEID ID of entity to be controlled if TYPE is not set to FUNCTION. If TYPE is set to FUNCTION, see Remark 5. For TYPE = POREAIR, TYPEID is the ID of the part containing material with pore air. TIMEOFF Flag for offset of time in curve: EQ.0: No offset is applied. EQ.1: Offset the abscissa of the time-dependent curve by the time value at which the sensor is triggered. Type Of Control Curve Affected PRESSURE PRESC-MOT PRESC-ORI *LOAD_SEGMENT *BOUNDARY_PRESCRIBED_MOTION *BOUNDARY_PRESCRIBED_ORIENTATION_RIGID Number of repeat of cycle of switches, SWITn, defined on the 2nd card. For example, a definition of SWITn like “601, 602, 601, 602, 601, 602” can be replaced by setting NREP to 3 and SWITn to ”601, 602”. Setting NREP = -1 repeats the cycle for infinite number of times. Default is 0. NREP VARIABLE ESTYP DESCRIPTION Type of element set to be controlled. With initial status set to “ON”, all the elements included in set TYPEID can be eroded when the controller status is changed to “OFF”. When TYPEID is not defined, all elements of type ESTYP in the whole system will be eroded. EQ.”BEAM”: Beam element set. EQ.”DISC”: Discrete element set EQ.”SHELL”: Thin shell element set EQ.”SOLID”: Solid element set EQ.”TSHELL”: Thick shell element set INITSTT Initial status: EQ.On: Initial status is on EQ.Off: Initial status is off ID of nth switch. At the start of the calculation SWIT1 is active, meaning that it controls the state of the feature specified in TYPEID. After SWIT1 triggers, then SWIT2 becomes active; after SWIT2 triggers, then SWIT3 becomes active; this process will continue until the entire stack of switches has been exhausted. SWITn Remarks: 1. Activation of Bag Venting. BAGVENTPOP activates (opens) or deactivates (closes) the venting holes of *AIRBAG_HYBRID and *AIRBAG_WANG_ NEFSKE. It overwrites the definitions of PVENT of *AIRBAG_HYBRID and PPOP of *AIRBAG_WANG_NEFSKE. More than one SWIT can be input to open/close initially closed/opened holes, and then reclose/reopen the holes. 2. Seatbelt Retractors. The locking (or firing) of seatbelt retractor (or preten- sioner) can be controlled through either general sensor, option BELTRETRA (or BELTPRET), or seatbelt sensors, *ELEMENT_SEATBELT_SENSOR. When BEL- TRETRA (or BELTPRET) is used, the SBSIDi in *ELEMENT_SEATBELT_RE- TRACTOR (or PRETENSIONER) should be left blank. 3. Seatbelt Slip Ring. For one-way slip ring, a non-zero DIRECT in *ELEMENT_- SEATBELT_SLIPRING, BELTSLIP activates the constraint of one-way slippage when the status of SENSOR_CONTROL is on. When the SENSOR_CONTROL is turned off, the one-way slippage constraint is deactivated, therefore allowing slippage in both directions. To model a two-way slip ring, BELTSLIP allow slippage in both directions when the status of SENSOR_CONTROL is on. When the status of SENSOR_- CONTROL is off, the slip ring lockup happens, no slippage is allowed then. 4. Switching Between Rigid and Deformable. DEF2RIG provides users more flexibility controlling material switch between rigid and deformable. Status of ON trigger the switch and deformable material becomes rigid. Rigidized mate- rial can then return to deformable status when status becomes OFF. As many as 7 SWITs can be input, any of them will change the status triggered by its preceding SWIT or the initial condition, INTSTT. 5. Function for Sensor Control. When the input parameter TYPE of *SENSOR_- CONTROL is set to "FUNCTION", the function "SENSOR(cntlid)" as described in *DEFINE_CURVE_FUNCTION takes on a value that depends on the current status of the *SENSOR_CONTROL. That status is either on or off at any given point in time. If the status is on, the value of function SENSOR(cntlid) is simply set to the integer value 1. If the status is off, the value of function SEN- SOR(cntlid) is set to the input parameter TYPEID (an integer) as specified in *SENSOR_CONTROL. To help clarify this relationship between *SENSOR_- CONTROL and *DEFINE_CURVE_FUNCTION, consider the following exam- ple. 6. Example of Function Sensor Control. Suppose a *SENSOR_CONTROL defined with CNTLID=101, TYPE="FUNCTION", and TYPEID = -2 has a status of off. Then a *DEFINE_CURVE_FUNCTION defined as “2+3*sensor(101)” will have a value of 2 + 3(-2) = -4. On the other hand, if the status of the *SEN- SOR_CONTROL changes to on, the *DEFINE_CURVE_FUNCTION takes on a value of 2 + 3(1) = 5. *SENSOR Purpose: This command will associate a CPM airbag with a sensor switch . When the condition flag is raised, the specified CPM airbag will deploy. All time dependent curves used for the CPM airbag are shifted by the activation time including the *AIRBAG_PARTICLE curves for the inflator and vent as well as the *MAT_FABRIC curves for TSRFAC. Card 1 1 2 3 4 5 6 7 8 Variable CPMID SWITID TBIRTH TDEATH TDR DEFPS RBPID Type I I F F F I I VARIABLE DESCRIPTION CPMID Bag ID of *AIRBAG_PARTICLE_ID SWITID Switch ID of *SENSOR_SWITCH TBIRTH If SWITID is set, TBIRTH is not active. If SWITID is 0, TBIRTH is the activation time for the bag with ID = CPMID. All of the time dependent curves that are used in this bag will be offset by the value of TBIRTH. TDEATH Disable the CPMID bag when the simulation time exceeds this value. TDR DEFPS If TDR is greater than 0 the bag with ID = CPMID will be rigid starting at first cycle and switch to deformable at time TDR. Part set ID specifiying which parts of the bag with ID = CPMID are deformable. RBPID Part ID of the master rigid body to which the part is merged. *SENSOR_DEFINE_CALC-MATH Purpose: Defines a new sensor with a unique ID. The values associated with this sensor are computed by performing mathematical calculations with the information obtained from sensors defined by the *SENSOR_DEFINE_OPTION. Math Sensor Cards. Include one additional card for each math sensor. This input ends at the next keyword (“*”) card. Card 1 2 3 4 5 6 7 8 Variable SENSID CALC SENS1 SENS2 SENS3 SENS4 SENS5 SENS6 Type I A I I I I I I VARIABLE DESCRIPTION SENSID Sensor ID. Mathematical calculation, See Table 37-2. ith Sensor ID CALC SENSi Remarks: All sensors, SENSi, defined with either SENSOR_DEFINE_NODE_SET or SENSOR_DE- FINE_ELEMENT_SET, must refer to either the same node set or the same element set. Example: $ $ assume set_2 to have 100 solid elements *SENSOR_DEFINE_ELEMENT_SET $ this sensor traces xx-strain of all 100 solid elements in set-2 91 SOLID -2 XX STRAIN *SENSOR_DEFINE_ELEMENT_SET $ this sensor traces yy-strain of all 100 solid elements in set-2 92 SOLID -2 YY STRAIN *SENSOR_DEFINE_ELEMENT_SET $ this sensor traces zz-strain of all 100 solid elements in set-2 93 SOLID -2 ZZ STRAIN *SENSOR_DEFINE_CALC-MATH $ this sensor traces strain magnitudes of all 100 solid elements in set-2 104 SQRTSQRE 91 92 93 0 0 0 *SENSOR_SWITCH $ Because ELEMID of *sensor_define_element_set was input as "-2", SWITCH-1 will be $ turned on if at least one of 100 elements has a strain magnitude>2.0E-4 $ On the other hand, If ELEMID was input as "2", SWITCH-1 will be turned on if $ all 100 elements have strain magnitudes>2.0E-4 1 SENSOR 104 GT 2.0E-4 0 0.001 $ ABSSUM MIN MAX MAXMAG MINMAG MULTIPLY *SENSOR_DEFINE_CALC-MATH *SENSOR FUNCTION DESCRIPTION Absolute value of the sum of sensor values MATHEMTAICAL FORM |SENS1 + SENS2 + ⋯ | The minimum of sensor values min(SENS1,SENS2, … ) The maximum of sensor values max(SENS1,SENS2, … ) The maximum of magnitude of sensor values The minimum of the magnitude of sensor values Multiplication of sensor values; negative for division (performed left to right) max(|SENS1|, |SENS2|, … ) min(|SENS1|, |SENS2|, … ) SENS1 × SENS2 × ⋯ SQRE Summation of squared values of sensor values SQRTSQRE Square root of the sum of squared values SENS12 + SENS22 + ⋯ √SENS12 + SENS22 + ⋯ SQRT Summation of square root of sensor values; negative for subtracting values √SENS1 + √SENS2 + ⋯ SUMABS Summation of absolute sensor values |SENS1| + |SENS2| + ⋯ SUM Summation of sensor values; negative for subtracting values SENS1 + SENS2 + ⋯ Table 37-2. Available mathematical functions. *SENSOR_DEFINE_ELEMENT_{OPTION} Available options include: <BLANK> SET Purpose: Define a strain gage type element sensor that checks the stress, strain, or resultant force of an element or element set. Element Sensor Cards. Include one additional card for each element sensor. This input ends at the next keyword (“*”) card. Card 1 2 3 4 5 6 Variable SENSID ETYPE ELEMID COMP CTYPE LAYER Type I A I A A A/I 7 SF R 8 PWR R Optional card for SET option. Card 1 2 3 4 5 6 7 8 Variable SETOPT Type A VARIABLE DESCRIPTION SENSID Sensor ID. ETYPE Element type. Available options include: EQ.BEAM: beam element. EQ.SHELL: shell element EQ.SOLID: solid element EQ.DISC-ELE: discrete element EQ.SEATBELT: seatbelt element EQ.TSHELL: thick shell element VARIABLE ELEMID DESCRIPTION Element ID or element set ID when option_SET is active. In case of option_SET, a positive ELEMID requires all elements in set EL- EMID to meet the switch condition to switch the status of related *SENSOR_SWITCH. If ELEMID is negative, the status of related *SENSOR_SWITCH will be changed if at least one of elements in set “-ELEMID” meets the switch condition. COMP Component type. The definition of component, and its related coordinate system, is consistent with that of elout. Leave blank for discrete elements. Available options for elements other than discrete element include: EQ.XX: EQ.YY: EQ.ZZ: EQ.XY: EQ.YZ: EQ.ZX: 𝑥-normal component for shells and solids 𝑦-normal component for shells and solids 𝑧-normal component for shells and solids 𝑥𝑦-shear component for shells and solids 𝑦𝑧-shear component for shells and solids 𝑧𝑥-shear component for shells and solids EQ.AXIAL: axial EQ.SHEARS: local 𝑠-direction EQ.SHEART: local 𝑡-direction CTYPE Sensor type. Available options include: EQ.STRAIN: strain component for shells and solids EQ.STRESS: stress component for shells and solids EQ.FORCE: resultants seatbelt, or force translational discrete element; moment resultant for rotational discrete element for beams, EQ.MOMENT: moment resultants for beams EQ.DLEN: change in length for discrete or seatbelt element EQ.FAIL: failure of element, sensor value = 1 when element fails, = 0 otherwise. LAYER *SENSOR_DEFINE_ELEMENT DESCRIPTION Layer of integration point in shell or thick shell element. Options include: EQ.BOT: component at lower surface meaning the integration point with the smallest through-the-thickness local coordinate EQ.TOP: component at upper surface meaning the integration point with the largest through-the-thickness local co- ordinate When CTYPE = STRESS, LAYER could be an integer “I” to monitor the stress of the I’the integration point. SF, PWR Optional parameters, scale factor and power, for users to adjust the resultant sensor value. The resultant sensor value is [SF × (Original Value)]PWR SETOPT Option to process set of data when SET option is specified. More details can be found in *SENSOR_DEFINE_NODE_SET. When SETOPT is defined, a single value will be reported, which could be EQ.AVG: the average value of the dataset EQ.MAX: the maximum value of the dataset EQ.MIN: the minimum value of the dataset EQ.SUM: the sum of the dataset Purpose: Define a force transducer type sensor. *SENSOR Force Sensor Cards. Include one additional card for each force sensor. This input ends at the next keyword (“*”) card. Card 1 2 3 4 5 6 7 8 Variable SENSID FTYPE TYPEID VID CRD Type I A I A/I I VARIABLE DESCRIPTION SENSID Sensor ID. FTYPE Force type. See Table 37-3. TYPEID ID defined in the associated KEYWORD command. See Table 37-3. VID Vector along which the forces is measured. EQ.X: EQ.Y: EQ.Z: 𝑥-direction in coordinate system CRD. 𝑦-direction in coordinate system CRD. 𝑧-direction in coordinate system CRD. EQ.XMOMENT: 𝑥-direction moment for JOINT, JOINTSTIF, PRESC-MOT or SPC. EQ.YMOMENT: 𝑦-direction moment for JOINT, JOINTSTIF, PRESC-MOT or SPC. EQ.ZMOMENT: 𝑧-direction moment for JOINT, JOINTSTIF, PRESC-MOT or SPC. VID∈{INT}: vector ID n in coordinate system CRD. CRD Optional coordinate system, defined by *DEFINE_COORDI- NATE_NODES, to which vector VID is attached. If blank the global coordinate system is assumed. FTYPE TYPEID (Enter ID defined in following KEYWORD commands) OUTPUT ASCII FILE AIRBAG *AIRBAG Airbag pressure ABSTAT CONTACT *CONTACT CONTACT2D *CONTACT_2D CPM *AIRBAG_PARTICLE JOINT *CONSTRAINED_JOINT JOINTSTIF *CONSTRAINED_JOINT_STIFFNESS PRESC-MOT *BOUNDARY_PRESCRIBED_MOTION RWALL *RIGIDWALL SPC *BOUNDARY_SPC Contact force on the slave side Contact force on the slave side Airbag pressure Joint force Joint stiffness force Prescribed motion force RCFORC RCFORC AB- STAT_CPM JNTFORC JNTFORC BNDOUT Rigid wall force RWFORC SPC reaction force SPCFORC SPOTWELD *CONSTRAINED_POINTS Spot weld force SWFORC X-SECTION *DATABASE_CROSS_SECTION Section force SECFORC Table 37-3. Force transducer type sensor *SENSOR Purpose: Defines a new sensor with a unique ID. The value associated with this sensor is computed by performing mathematical calculations defined in *DEFINE_FUNC- TION, with the information obtained from other sensors defined by the *SENSOR_DE- FINE_OPTION. Card 1 1 2 3 4 5 6 7 8 Variable SENSID FUNC SENS1 SENS2 SENS3 SENS4 SENS5 SENS6 Type I I I I I I I I Sensor Cards. Additional Cards needed when SENS1 < -5. Include as many cards as needed to specify all |SENS1| cards. Card 2 1 2 3 4 5 6 7 8 Variable SENSi SENSi+1 SENSi+2 SENSi+3 SENSi+4 SENSi+5 SENSi+6 SENSi+7 Type I I I I I I I I VARIABLE DESCRIPTION SENSID Sensor ID FUNC SENS1 Function ID 1st Sensor ID, the value of which will be used as the 1st argument of function FUNC. If defined as negative, the absolute value of SENS1, |SENS1|, is the number of sensors to be input. If |SENS1| > 5, additional cards will be needed to input the ID of all sensors. The number of sensor is limited to 15. SENSi ith Sensor ID, the value of which will be used as the ith argument of function FUNC *SENSOR_DEFINE_MISC Purpose: Trace the value of a miscellaneous item. This card replaces *SENSOR_DE- FINE_ANGLE. Force Sensor Cards. Include one additional card for each miscellaneous sensor. This input ends at the next keyword (“*”) card. Card 1 2 3 Variable SENSID MTYPE 4 I1 5 I2 6 I3 7 I4 8 I5 Type I A I/A I/A I/A I/A I/A VARIABLE DESCRIPTION SENSID Sensor ID. VARIABLE DESCRIPTION MTYPE Entity to be traced: EQ.ANGLE: Angular accelerometer sensor tracing the angle between two lines, 0≤ θ ≤180. The fields I1 and I2 are node numbers defining the 1st line, while I3 and I4 are node num- bers defining the 2nd line. EQ.CURVE: The value of a time-dependent curve defined or by *DEFINE_CURVE_FUNCTION *DEFINE_CURVE. I1 is the curve ID. EQ.RETRACTOR: The seatbelt retractor payout rate is traced. I1 is the retractor ID. EQ.RIGIDBODY: Accelerometer sensor tracing the kinematics of a rigid body with id I1. The I2 field speci- fies which kinematical component is to be traced. It may be set to “TX”, “TY”, or “TZ” for 𝑋, 𝑌, and 𝑍 translations and to “RX”, “RY”, or “RZ” for the 𝑋, 𝑌, and 𝑍 compo- nents of the rotation. The I3 field specifies the kinematics type: “D” for displacement, “V” for velocity and “A” for acceleration. Output is calculated with respect to the global coordinate system when the I4 field is set to “0”, its default value; the local rigid- body coordinate system is used when I4 is set to “1”. EQ.TIME: The current analysis time is traced. I1, …, I5 See MTYPE. *SENSOR_DEFINE_NODE_{OPTION} Available options include: <BLANK> SET Purpose: Define an accelerometer type sensor. This command outputs the relative linear acceleration, velocity, or relative coordinate of node-1 with respect to node-2 along vector VID. Node Sensor Cards. Include one additional card for each node sensor. This input ends at the next keyword (“*”) card. Card 1 2 3 4 5 6 7 8 Variable SENSID NODE1 NODE2 VID CTYPE SETOPT Type I I I I A A VARIABLE DESCRIPTION SENSID Sensor ID. NODE1,2 Nodes defining the accelerometer. NODE1 is a node set ID when option_SET is active. In case of option_SET, and when SETOPT is not defined, a positive NODE1 requires all nodes in set NODE1 to meet the switch condition to switch the status of related *SEN- SOR_SWITCH. If NODE1 is negative, the status of related *SEN- SOR_SWITCH will be changed if at least one of nodes in set “- NODE1” meets the switch condition. VID ID of vector along which the nodal values are measured, see *DE- FINE_VECTOR. The magnitude of nodal values (coordinate, velocity or acceleration) will be output if VID is 0 or undefined. CTYPE Output component type (character string). EQ.ACC: acceleration EQ.VEL: velocity EQ.COORD: coordinate EQ.TEMP: temperature VARIABLE SETOPT DESCRIPTION Option to process set of data when SET option is specified. When SETOPT is specified, a single value will be reported, which could be EQ.AVG: the average value of the dataset EQ.MAX: the maximum value of the dataset EQ.MIN: the minimum value of the dataset EQ.SUM: the sum of the dataset Remarks: 1. Time Evolution of Vector VID. The vector direction is determined by *DE- FINE_VECTOR. This vector direction is updated with time only if the coordi- nate system CID is defined using *DEFINE_COORDI- NATE_NODES and the parameter FLAG is set to 1. Otherwise, the vector direction is fixed. 2. SETOPT. When SETOPT is not defined for SET option, a list of nodal data will be reported, one for each node in the node set. These reported nodal values can be processed by *SENSOR_DEFINE_FUNCTION and *SENSOR_DEFINE_- CALC-MATH, and then result in a list of processed values. These nodal values can be used to determine if the status of SENSOR_SWITCH will be changed. Depending on the sign of NODE1, it can take only one single data point or the whole data sets to meet the switch condition to change the status of the related SENSOR_SWITCH. It should be note that all sensor definitions referred to by these two processing commands must have the same number of data points. The reported nodal values cannot be accessed by commands like *DEFINE_- CURVE_FUNCTION, see SENSORD option. When SETOPT is defined, the nodal values of all nodes in the node set will be processed, depending on the definition of SETOPT, the resulting value is re- ported as the single sensor value. The reported value can be processed by both *SENSOR_DEFINE_FUNCTION and *SENSOR_DEFINE_CALC-MATH as well as other regular sensors. This reported value can also be accessed by * DE- FINE_CURVE_FUNCTION using SENSORD option. If the reference node, node2, is needed, NODE2 has to be a node set containing the same number of nodes as node set “-NODE1”. The nodes in sets “-NODE1” and “NODE2” have to be arranged in the same sequence so that the nodal value of nodes in set “- NODE1” can be measured with respect to the correct node in set NODE2. 3. When NODE1 is a node that belongs to a rigid body and CTTYPE=”ACC”, the acceleration recorded by the sensor is not updated every time step but rather only when nodal output is written according to *DATABASE commands. As an alternative, *SENSOR_DEFINE_MISC with MTYPE=”RIGIDBODY” up- dates the sensor data every time step. *SENSOR Purpose: This command compares the value of a sensor, *SENSOR_DEFINE or SEN- SOR_CALC-MATH, to a given criterion to check if the switch condition is met. It output a logic value of TRUE or FALSE. Sensor Switch Cards. Include one additional card for each sensor switch. This input ends at the next keyword (“*”) card. Card 1 1 2 3 4 5 6 7 8 Variable SWITID SENSID LOGIC VALUE FILTRID TIMWIN Type I I A F I F VARIABLE SWITID DESCRIPTION Switch ID can be referred directly by *SENSOR_CONTROL to control the status of entities like CONTACT and AIRBAG, or can be referred to by *SENSOR_SWITCH_CALC-LOGIC for logic computation. SENSID ID of the sensor whose value will be compared to the criterion to determine if a switch condition is met. LOGIC Logic operator, could be either LT (<) or GT (>). VALUE Critical value FILTER TIMWIN Filter ID (optional). Filters may be defined using *DEFINE_FIL- TER. Trigger a status change when the value given by the sensor is less than or greater than (depending on LOGIC) the VALUE for a duration defined by TIMWIN. *SENSOR_SWITCH_CALC-LOGIC Purpose: This command performs a logic calculation for the logic output of up to seven *SENSOR_SWITCH or *SENSOR_SWITCH_CALC-LOGIC definitions. The output is a logic value of either TRUE or FALSE. Log Cards. Include one additional card for each logic rule. This input ends at the next keyword (“*”) card. Card 1 2 3 4 5 6 7 8 Variable SWITID SWIT1 SWIT2 SWIT3 SWIT4 SWIT5 SWIT6 SWIT7 Type I I I I I I I I VARIABLE SWITID DESCRIPTION Switch ID can be referred directly by *SENSOR_CONTROL to control the status of entities like CONTACT and AIRBAG, or can be referred to by *SENSOR_SWITCH_CALC-LOGIC for logic computation. SWITn Input a positive sensor switch ID for "AND" and negative sensor switch ID for "OR". SWIT1 must always be positive. This keyword implements standard Boolean logic. true = 1, false = 0, and = multiplication, or = addition An expression evaluating to 0 is false, while any expression that evaluates to greater than 0 is true, and, therefore, set to 1. Example: Consider 5 switches defined as follows: switch(11) = true switch(12) = false switch(13) = true switch(14) = true To evaluate the expression switch(15) = false. [switch(11) or switch(12) or switch(13)] and [switch(14) or switch(15)] and assign the value to switch(103), the following would apply: *SENSOR_SWITCH_CALC-LOGIC 101,11,-12,-13 102,14,-15 103,101,102 This translates into switch(101) = switch(11) or switch(12) or switch(13) = min((1 + 0 + 1), 1) = 1 (true) switch(102) = switch(14) or switch(15) = min((1 + 0), 1) = 1 (true) switch(103) = switch(101) and switch(102) = min((1 × 1), 1) = 1 (true) Therefore, switch(101)=true ⏞⏞⏞⏞⏞⏞⏞⏞⏞⏞⏞⏞⏞⏞⏞⏞⏞⏞⏞⏞⏞ [switch(11) or 𝑠witch(12) or switch(13)] switch(102)=true ⏞⏞⏞⏞⏞⏞⏞⏞⏞⏞⏞⏞⏞ AND [switch(14) or switch(15)] = switch(103) = true *SENSOR_SWITCH_SHELL_TO_VENT Purpose: This option will treat the failed shell elements as vent hole for the airbag defined by *AIRBAG_PARTICLE. The mass escaped from the vent will be reported in abstat_cpm file. Card 1 Variable 1 ID 2 3 4 5 6 7 8 ITYPE C23 Type I I F Shell Fail Time Cards. Optional Cards for setting time at which shells in a shell list change into vents. This card may be repeated up time 15 times. This input ends at the next keyword (“*”) cards. Optional 1 2 3 4 5 6 7 8 Variable SSID FTIME C23V Type I F F Default none 0. C23 VARIABLE DESCRIPTION ID TYPE Part set ID/Part ID. EQ.0: Part EQ.1: Part set C23 Vent Coefficient (Default = 0.7) LT.0: User defined load curve ID. The vent coefficient will be determined by this pressure-vent_coeff curve. SSID ID of *SET_SHELL_LIST FTIME Time to convert shell list to vent. (Default is from t = 0.) VARIABLE DESCRIPTION C23V Vent Coefficient (Default = C23) LT.0: User defined load curve ID. The vent coefficient will be determined by this pressure-vent_coeff curve. The keyword *SET provides a convenient way of defining groups of nodes, parts, elements, and segments. The sets can be used in the definitions of contact interfaces, loading conditions, boundary conditions, and other inputs. The keyword provides also a convenient way of defining groups of vibration modes to be used in frequency domain analysis. Each set type must have a unique numeric identification. The keyword control cards in this section are defined in alphabetical order: *SET_BEAM_{OPTION}_{OPTION} *SET_BEAM_ADD *SET_BEAM_INTERSECT *SET_BOX *SET_DISCRETE_{OPTION}_{OPTION} *SET_DISCRETE_ADD *SET_MODE_{OPTION} *SET_MULTIMATERIAL_GROUP_LIST *SET_NODE_{OPTION}_{OPTION} *SET_NODE_ADD_{OPTION} *SET_NODE_INTERSECT *SET_PART_{OPTION}_{OPTION} *SET_PART_ADD *SET_SEGMENT_{OPTION}_{OPTION} *SET_SEGMENT_ADD *SET_SEGMENT_INTERSECT *SET_2D_SEGMENT_{OPTION}_{OPTION} *SET_SHELL_{OPTION}_{OPTION} *SET_SHELL_ADD *SET_SHELL_INTERSECT *SET_SOLID_ADD *SET_SOLIDT_INTERSECT *SET_TSHELL_{OPTION}_{OPTION} An additional option_TITLE may be appended to all the *SET keywords. If this option is used then an addition line is read for each section in 80a format which can be used to describe the set. At present LS-DYNA does make use of the title. Inclusion of titles gives greater clarity to input decks. The GENERAL option is available for set definitions. In this option, the commands are executed in the order defined. For example, the delete option cannot delete a node or element unless the node or element was previously added via a command such as BOX or ALL. The COLLECT option allows for the definition of multiple sets that share the same ID and combines them into one large set whenever this option is found. If two or more like sets definitions share the same IDs, they are combined if and only if the_COLLECT option is specified in each definition. If the_COLLECT option is not specified for one or more like set definitions that share identical ID’s an error termination will occur. For include files using *INCLUDE_TRANSFORM where set offsets are specified, the offsets are not applied for the case where the_COLLECT option is present. *SET_BEAM_{OPTION1}_{OPTION2} For OPTION1 the available options are: <BLANK> GENERATE GENERATE_INCREMENT GENERAL For OPTION2 the available option is: COLLECT The GENERATE and GENERATE_INCREMENT options will generate block(s) of beam element ID’s between a starting ID and an ending ID. An arbitrary number of blocks can be specified to define the set. Purpose: Define a set of beam elements or a set of seat belt elements . Card 1 1 2 3 4 5 6 7 8 Variable SID Type I Default none Beam Element ID Cards. This Card 2 format applies to the case of an unset (<BLANK>) keyword option. Set one value per element in the set. Include as many cards as needed. This input ends at the next keyword (“*”) card. Card 2 Variable 1 K1 Type I 2 K2 I 3 K3 I 4 K4 I 5 K5 I 6 K6 I 7 K7 I 8 K8 Beam Element Range Cards. This Card 2 format applies to the GENERATE keyword option. Set one pair of BNBEG and BNEND values per block of elements. Include as many cards as needed. This input ends at the next keyword (“*”) card. Card 2 1 2 3 4 5 6 7 8 Variable B1BEG B1END B2BEG B2END B3BEG B3END B4BEG B4END Type I I I I I I I I Beam Element Range with Increment Cards. This Card 2 format applies to the GEN- ERATE_INCREMENT keyword option. For each block of elements add one card to the deck. This input ends at the next keyword (“*”) card. Card 2 1 2 3 4 5 6 7 8 Variable BBEG BEND INCR Type I I I Generalized Beam Element Range Cards. This Card 2 format applies to the GENERAL keyword option. Include as many cards as needed. This input ends at the next keyword (“*”) card. Card 2… 1 Variable OPTION Type A 2 E1 I 3 E2 I 4 E3 I 5 E4 I 6 E5 I 7 E6 I 8 E7 I VARIABLE DESCRIPTION SID K1 K2 ⋮ Set ID First beam element Second beam element ⋮ B[N]BEG First beam element ID in block N. B[N]END BBEG BEND INCR *SET DESCRIPTION Last beam element ID in block N. All defined ID’s between and including B[N]BEG to B[N]END are added to the set. These sets are generated after all input is read so that gaps in the element numbering are not a problem. B[N]BEG and B[N]END may simply be limits on the ID’s and not element ID’s. First beam element ID in block. Last beam element ID in block. Beam ID increment. Beam IDs BBEG, BBEG + INCR, BBEG + 2 × INCR, and so on through BEND are added to the set. OPTION Option for GENERAL. See table below. E1, …, E7 Specified entity. Each card must have the option specified. See table below. The General Option: The “OPTION” column in the table below enumerates the allowed values for the “OPTION” variable in Card 2 for the GENERAL option. Likewise, the variables E1, …, E7 refer to the GENERAL option Card 2. Each of the following operations accept up to 7 arguments, but they may take fewer. Values of “En” left unspecified are ignored. OPTION ALL ELEM DESCRIPTION All beam elements will be included in the set. Elements E1, E2, E3, ... will be included. DELEM Elements E1, E2, E3, ... previously added will be excluded. PART Elements of parts E1, E2, E3, ... will be included. DPART BOX DBOX Elements of parts E1, E2, E3, ... previously added will be excluded. Elements inside boxes E1, E2, E3, ... will be included. Elements inside boxes E1, E2, E3, ... previously added will be excluded. *SET_BEAM_ADD Purpose: Define a beam set by combining beam sets. Card 1 1 2 3 4 5 6 7 8 Variable SID Type I Default none Beam Element Set Cards. Each card can be used to specify up to 8 beam element sets. Include as many cards of this kind as necessary. This input ends at the next keyword (“*”) card. Card 2 1 2 3 4 5 6 7 8 Variable BSID1 BSID2 BSID3 BSID4 BSID5 BSID6 BSID7 BSID8 Type I I I I I I I I VARIABLE SID DESCRIPTION Set ID of new beam set. All beam sets should have a unique set ID. BSID[N] The Nth beam set ID on the card *SET Purpose: Define a beam set as the intersection, ∩, of a series of beam sets. The new beam set, SID, contains only the elements common to of all beam sets listed on the cards of format 2. Card 1 1 2 3 4 5 6 7 8 Variable SID Type I Default none Beam Set Cards. Each card can be used to specify up to 8 beam sets. Include as many cards of this kind as necessary. This input ends at the next keyword (“*”) card. Card 2 1 2 3 4 5 6 7 8 Variable BSID1 BSID2 BSID3 BSID4 BSID5 BSID6 BSID7 BSID8 Type I I I I I I I I VARIABLE SID DESCRIPTION Set ID of new beam set. All beam sets should have a unique set ID. BSID[N] The Nth beam set ID on card2 *SET_BOX Purpose: Define a set of boxes. The new box set, SID, contains a set of box IDs listed on the cards of format 2. Refer box ID in *DEFINE_BOX. Card 1 1 2 3 4 5 6 7 8 Variable SID Type I Default none Box Set Cards. Each card can be used to specify up to 8 box IDs. Include as many cards of this kind as necessary. This input ends at the next keyword (“*”) card. Card 2 1 2 3 4 5 6 7 8 Variable BID1 BID2 BID3 BID4 BID5 BID6 BID7 BID8 Type I I I I I I I I VARIABLE DESCRIPTION SID Set ID of new box set. All box sets should have a unique set ID. BID[N] The Nth box ID on card2 *SET_DISCRETE_{OPTION1}_{OPTION2} For OPTION1 the available options are: <BLANK> GENERATE GENERAL For OPTION2 the available option is: COLLECT The option GENERATE will generate a block of discrete element ID’s between a starting ID and an ending ID. An arbitrary number of blocks can be specified to define the set. Purpose: Define a set of discrete elements. Card 1 1 2 3 4 5 6 7 8 Variable SID Type I Default none Discrete Element ID Cards. This Card 2 format applies to the case of an unset (<BLANK>) keyword option. Set one value per element in the set. Include as many cards as needed. This input ends at the next keyword (“*”) card. Card 2 Variable 1 K1 Type I 2 K2 I 3 K3 I 4 K4 I 5 K5 I 6 K6 I 7 K7 I 8 K8 Discrete Element Range Cards. This Card 2 format applies to the GENERATE keyword option. Set one pair of BNBEG and BNEND values per block of elements. Include as many cards as needed. This input ends at the next keyword (“*”) card. Card 2 1 2 3 4 5 6 7 8 Variable B1BEG B1END B2BEG B2END B3BEG B3END B4BEG B4END Type I I I I I I I I Generalized Discrete Element Range Cards. This Card 2 format applies to the GENERAL keyword option. Include as many cards as needed. This input ends at the next keyword (“*”) card. Card 2 1 Variable OPTION Type A 2 E1 I 3 E2 I 4 E3 I 5 E4 I 6 E5 I 7 E6 I 8 E7 I VARIABLE DESCRIPTION SID K1 K2 ⋮ Set ID First discrete element Second discrete element ⋮ B[N]BEG First discrete element ID in block N. B[N]END Last discrete element ID in block N. All defined ID’s between and including B[N]BEG to B[N]END are added to the set. These sets are generated after all input is read so that gaps in the element numbering are not a problem. B[N]BEG and B[N]END may simply be limits on the ID’s and not element ID’s. OPTION Option for GENERAL. See table below. E1, …, E7 Specified entity. Each card must have the option specified. See table below. *SET The “OPTION” column in the table below enumerates the allowed values for the “OPTION” variable in Card 2 for the GENERAL option. Likewise, the variables E1, …, E7 refer to the GENERAL option Card 2. Each of the following operations accept up to 7 arguments, but they may take fewer. Values of “En” left unspecified are ignored. OPTION ALL ELEM DESCRIPTION All discrete elements will be included in the set. Elements E1, E2, E3, ... will be included. DELEM Elements E1, E2, E3, ... previously added will be excluded. PART Elements of parts E1, E2, E3, ... will be included. DPART BOX DBOX Elements of parts E1, E2, E3, ... previously added will be excluded. Elements inside boxes E1, E2, E3, ... will be included. Elements inside boxes E1, E2, E3, ... previously added will be excluded. *SET_DISCRETE_ADD Purpose: Define a discrete set by combining discrete sets. Card 1 1 2 3 4 5 6 7 8 Variable SID Type I Default none Discrete Element Set Cards. Each card can be used to specify up to 8 discrete element sets. Include as many cards of this kind as necessary. This input ends at the next keyword (“*”) card. Card 2 1 2 3 4 5 6 7 8 Variable DSID1 DSID2 DSID3 DSID4 DSID5 DSID6 DSID7 DSID8 Type I I I I I I I I VARIABLE SID DESCRIPTION Set ID of new discrete element set. All discrete element sets must have a unique ID. DSID[N] The Nth discrete set ID on card2 Available options include: <BLANK> LIST LIST_GENERATE *SET The last option, LIST_GENERATE, will generate a block of mode ID’s between a starting ID and an ending ID. An arbitrary number of blocks can be specified to define the set. Purpose: Define a set of modes. Card 1 1 2 3 4 5 6 7 8 Variable SID Type I Default none Mode ID Cards. This Card 2 format applies to the for keyword option set to LIST or for an unset (<BLANK>) keyword option. Set one value per mode in the set. Include as many cards as needed. This input ends at the next keyword (“*”) card. Card 2 1 2 3 4 5 6 7 8 Variable MID1 MID2 MID3 MID4 MID5 MID6 MID7 MID8 Type I I I I I I I Mode Range Cards. This Card 2 format applies to the GENERATE keyword option. Set one pair of BNBEG and BNEND values per block of modes. Include as many cards as needed. This input ends at the next keyword (“*”) card. Card 2 1 2 3 4 5 6 7 8 Variable M1BEG M1END M2BEG M2END M3BEG M3END M4BEG M4END Type I I I I I I I I VARIABLE DESCRIPTION SID Set identification. All mode sets should have a unique set ID. MID[N] Mode ID N. M[N]BEG First mode ID in block N. M[N]END Last mode ID in block N. All defined ID’s between and including M[N]BEG and M[N]END are added to the set. Remarks: 1. The available mode ID’s can be found in ASCII file eigout, or binary database d3eigv. *SET_MULTI Note that this keyword’s name has been shortened. Its older long form, however, is still also valid. *SET_MULTI-MATERIAL_GROUP_LIST Purpose: This command defines an ALE multi-material set ID (AMMSID) which contains a collection of one or more ALE multi-material group ID(s) (AMMGID). This provides a means for selecting any specific ALE multi-material(s). Application includes, for example, a selection of any particular fluid(s) to be coupled to a fluid- structure interaction. Card 1 1 2 3 4 5 6 7 8 Variable AMSID Type Default I 0 Multi-Material Group ID Cards. Set one value per element in the set. Include as many cards as needed. This input ends at the next keyword (“*”) card. Card 2 1 2 3 4 5 6 7 8 Variable AMGID1 AMGID2 AMGID3 AMGID4 AMGID5 AMGID6 AMGID7 AMGID8 Type Default I 0 I 0 I 0 I 0 I 0 I 0 I 0 I 0 VARIABLE AMSID DESCRIPTION An ALE multi-material set ID (AMSID) which contains a collection of one or more ALE multi-material group ID(s) (AMGID). AMGID1 The 1st ALE multi-material group ID (AMGID = 1) defined by the 1st data line of the *ALE_MULTI-MATERIAL_GROUP card. ⋮ ⋮ *SET_MULTI-MATERIAL_GROUP_LIST DESCRIPTION The 8th ALE multi-material group ID (AMGID = 1) defined by the 8th data line of the *ALE_MULTI-MATERIAL_GROUP card. *SET VARIABLE AMGID8 Remarks: 1. Refer to an example in the *CONSTRAINED_LAGRANGE_IN_SOLID section. *SET_NODE_{OPTION1}_{OPTION2} For OPTION1 the available options are: <BLANK> LIST COLUMN LIST_GENERATE LIST_GENERATE_INCREMENT GENERAL LIST_SMOOTH For OPTION2 the available option is: COLLECT The LIST option generates a set for a list of node IDs. The LIST_GENERATE and LIST_- GENERATE_INCREMENT options will generate block(s) of node IDs between a starting ID and an ending ID. An arbitrary number of blocks can be specified to define the node set. The option LIST_SMOOTH is used to define a local region on a distorted tooling mesh to be smoothed. The LIST_SMOOTH option is documented in the Local smoothing of tooling mesh section of the *INTERFACE_COMPENSATION_NEW card’s documentation. The COLUMN option is for setting nodal attributes, which pass data to other keyword cards, on a node-by-node basis. Purpose: Define a nodal set with some identical or unique attributes. Card 1 1 2 3 4 5 6 7 8 Variable SID DA1 DA2 DA3 DA4 SOLVER Type I F Default none 0. Remark 1 F 0. 1 F 0. 1 F A 0. MECH 1 Node ID Cards. This Card 2 format applies to LIST and LIST_SMOOTH keyword options. Additionally, it applies to the case of an unset (<BLANK>) keyword option. Set one value per node in the set. Include as many cards as needed. This input ends at the next keyword (“*”) card. Card 2 1 2 3 4 5 6 7 8 Variable NID1 NID2 NID3 NID4 NID5 NID6 NID7 NID8 Type I I I I I I I I Node ID with Column Cards. This Card 2 format applies to the COLUMN keyword option. Include one card per node in the set. Include as many cards as needed. This input ends at the next keyword (“*”) card. Card 2 1 Variable NID Type I Remark 2 A1 F 2 3 A2 F 2 4 A3 F 2 5 A4 F 2 6 7 8 Node ID Range Cards. This Card 2 format applies to the LIST_GENERATE keyword option. Set one pair of BNBEG and BNEND values per block of nodes. Include as many cards as needed. This input ends at the next keyword (“*”) card. Card 2 1 2 3 4 5 6 7 8 Variable B1BEG B1END B2BEG B2END B3BEG B3END B4BEG B4END Type I I I I I I I Node ID Range with Increment Cards. This Card 2 format applies to the LIST_GEN- ERATE_INCREMENT keyword option. For each block of nodes add one card to the deck. This input ends at the next keyword (“*”) card. Card 2 1 2 3 4 5 6 7 8 Variable BBEG BEND INCR Type I I I Generalized Node ID Range Cards. This Card 2 format applies to the GENERAL keyword option. Include as many cards as needed. This input ends at the next keyword (“*”) card. Card 2 1 Variable OPTION Type A 2 E1 I 3 E2 I 4 E3 I 5 E4 I 6 E5 I 7 E6 I 8 E7 I VARIABLE DESCRIPTION SID DA1 DA2 DA3 DA4 Set identification. All node sets should have a unique set ID. First nodal attribute default value, see remark 1 below. Second nodal attribute default value Third nodal attribute default value Fourth nodal attribute default value SOLVER Name of solver using this set (MECH, CESE, etc.) NIDi NID A1 A2 A3 A4 Node ID i Nodal ID First nodal attribute, see remark 2 below. Second nodal attribute Third nodal attribute Fourth nodal attribute VARIABLE DESCRIPTION BnBEG First node ID in block n. BnEND BBEG BEND INCR Last node ID in block n. All defined ID’s between and including BnBEG to BnEND are added to the set. These sets are generated after all input is read so that gaps in the node numbering are not a problem. BnBEG and BnEND may simply be limits on the ID’s and not nodal ID’s. First node ID in block. Last node ID in block. Node ID increment. Node IDs BBEG, BBEG + INCR, BBEG + 2 × INCR, and so on through BEND are added to the set. OPTION Option for GENERAL. See table below. E1, …, E7 Specified entity. Each card must have the option specified. See table below. The General Option: The “OPTION” column in the table below enumerates the allowed values for the “OPTION” variable in Card 2 for the GENERAL option. Likewise, the variables E1, …, E7 refer to the GENERAL option Card 2. Each of the following operations accept up to 7 arguments, but they may take fewer. Values of “En” left unspecified are ignored. OPTION DESCRIPTION ALL All nodes will be included in the set. NODE Nodes E1, E2, E3, … will be included. DNODE Nodes E1, E2, E3, … previously added will be excluded. PART Nodes of parts E1, E2, E3, … will be included. DPART Nodes of parts E1, E2, E3, … previously added will be excluded. BOX Nodes inside boxes E1, E2, E3, … will be included. DBOX VOL DVOL SET_XXXX SALECPT *SET DESCRIPTION Nodes inside boxes E1, E2, E3, … previously added will be excluded. Nodes inside contact volumes E1, E2, E3, … will be included. Nodes inside contact volumes E1, E2, E3, … previously added will be excluded. Include nodal points of element sets defined by SET_XXXX_ LIST, where XXXX could be SHELL, SOLID, BEAM, TSHELL and SPRING Nodes inside a box in Structured ALE mesh. E1 here is the S-ALE mesh ID (MSHID). E2, E3, E4, E5, E6, E7 correspond to XMIN, XMAX, YMIN, YMAX, ZMIN, ZMAX. They are the minimum and the maximum nodal indices along each direction in S-ALE mesh. This option is only to be used for Structured ALE mesh and should not be used in a mixed manner with other “_GENER- AL” options. refer Please *ALE_STRUCTURED_MESH_CONTROL_- POINTS and *ALE_STRUCTURED_MESH_CONTROL for more details. to SALEFAC Nodes that are on the face of a Structured ALE mesh. E1 gives the S-ALE mesh ID (MSHID). E2, E3, E4, E5, E6, E7 correspond to -𝑥, +𝑥, -𝑦, +𝑦, -𝑧, +𝑧 faces. Assigning 1, for instance, to these 6 values would include all the surface segments at these faces in the segment set. This option is only to be used for Structured ALE mesh and should not be used in a mixed manner with other “_GENERAL” options. refer *ALE_STRUCTURED_MESH_CONTROL_- Please POINTS and *ALE_STRUCTURED_MESH_CONTROL for more details. to Remarks: 1. Nodal attributes can be assigned to pass data to other keywords. For example, for contact option, *CONTACT_TIEBREAK_NODES_TO_SURFACE the attrib- utes are: DA1 = NFLF ⇒ Normal failure force, DA2 = NSFL ⇒ Shear failure force, DA3 = NNEN ⇒ Exponent for normal force, DA4 = NMES ⇒ Exponent for shear force. 2. The default nodal attributes can be overridden on these cards; otherwise, A1 = DA1, etc. 3. This field is used by a non-mechanics solver to create a set defined on that solver’s mesh. By default, the set refers to the mechanics mesh. 4. The option *SET_NODE_LIST_SMOOTH is used for localized tooling surface smoothing, and is used in conjunction with keywords *INTERFACE_COM- PENSATION_NEW_LOCAL_SMOOTH, *INCLUDE_COMPENSATION_- ORIGINAL_RIGID_TOOL, and *INCLUDE_COMPENSATION_NEW_RIGID_- TOOL. This option is available in R6 Revision 73850 and later releases Available options include: <BLANK> ADVANCED *SET Purpose: Define a node set by combining node sets or for the ADVANCED option by combining, NODE, SHELL, SOLID, BEAM, SEGMENT, DISCRETE and THICK SHELL sets. Card 1 1 2 3 4 5 6 7 8 Variable NSID DA1 DA2 DA3 DA4 SOLVER Type I F F F F A Default none none none none none MECH Remark 1 Node Set Cards. This Card 2 format is used when the keyword option is left unset (<BLANK>). Each card can be used to specify up to 8 node set IDs. Include as many cards of this kind as necessary. This input ends at the next keyword (“*”) card. Card 2 1 2 3 4 5 6 7 8 Variable NSID1 NSID2 NSID3 NSID4 NSID5 NSID6 NSID7 NSID8 Type I I I I I I I Node Set Advanced Cards. This Card 2 format is used when the keyword option is set to ADVANCED. Each card can be used to specify up to 4 set IDs (node sets, beam sets, etc…). Include as many cards of this kind as necessary. This input ends at the next keyword (“*”) card. Card 2 1 2 3 4 5 6 7 8 Variable SID1 TYPE1 SID2 TYPE2 SID3 TYPE3 SID4 TYPE4 Type I I I I I I I I VARIABLE DESCRIPTION NSID DA1 DA2 DA3 DA4 Set ID of new node set. All node sets should have a unique set ID. First nodal attribute default value, see remark 1 below. Second nodal attribute default value Third nodal attribute default value Fourth nodal attribute default value SOLVER Name of solver using this set (MECH, CESE, etc.) NSID[N] The Nth node set ID on Card 2 in LIST format. SID[N] The Nth set ID on Card 2 in ADVANCED format. TYPE[N] Type set for SID[N]: EQ.1: Node set EQ.2: Shell set EQ.3: Beam set EQ.4: Solid set EQ.5: Segment set EQ.6: Discrete set EQ.7: Thick shell set *SET 1. This field is used by a non-mechanics solver to create a set defined on that solver’s mesh. By default, the set refers to the mechanics mesh. *SET_NODE_INTERSECT Purpose: Define a node set as the intersection, ∩, of a series of node sets. The new node set, NSID, contains all common elements of all node sets listed on all cards in format 2. Card 1 1 2 3 4 5 6 7 8 Variable SID DA1 DA2 DA3 DA4 SOLVER Type I F F F F A Default none none none none none MECH Remark 1 Node Set Cards. For each SID in the intersection specify one field. Include as many cards as necessary. This input ends at the next keyword (“*”) card. Card 2 1 2 3 4 5 6 7 8 Variable NSID1 NSID2 NSID3 NSID4 NSID5 NSID6 NSID7 NSID8 Type I I I I I I I I VARIABLE SID DESCRIPTION Set ID of new node set. All node sets should have a unique set ID. DAi Nodal attribute of the i’th node. SOLVER Name of solver using this set (MECH, CESE, etc.) NSIDn The nth node set ID. Remarks: 1. This field is used by a non-mechanics solver to create a set defined on that solver’s mesh. By default, the set refers to the mechanics mesh. *SET_PART_{OPTION1}_{OPTION2} For OPTION1 available options are: <BLANK> LIST COLUMN LIST_GENERATE LIST_GENERATE_INCREMENT For OPTION2 the available option is: COLLECT The LIST_GENERATE and LIST_GENERATE_INCREMENT options will generate block(s) of part IDs between a starting ID and an ending ID. An arbitrary number of blocks can be specified to define the part set. Purpose: Define a set of parts with optional attributes. For the column option, see *AIRBAG or *CONSTRAINED_RIGID_BODY_STOPPERS. Card 1 1 2 3 4 5 6 7 8 Variable SID DA1 DA2 DA3 DA4 SOLVER Type I F F F F A Default none 0. MECH Remark 1 1 1 1 Part ID Cards. This Card 2 format applies to the LIST keyword option. Additionally, it applies to the case of an unset (<BLANK>) keyword option. Set one value per part in the set. Include as many cards as needed. This input ends at the next keyword (“*”) card. Card 2 1 2 3 4 5 6 7 8 Variable PID1 PID2 PID3 PID4 PID5 PID6 PID7 PID8 Type I I I I I I I I Part ID with Column Cards. This Card 2 format applies to the COLUMN keyword option. Include one card per part in the set. Include as many cards as needed. This input ends at the next keyword (“*”) card. Card 2 1 Variable PID Type I Remark 2 A1 F 2 3 A2 F 2 4 A3 F 2 5 A4 F 2 6 7 8 Part ID Range Cards. This Card 2 format applies to the GENERATE keyword option. Set one pair of BNBEG and BNEND values per block of part IDs. Include as many cards as needed. This input ends at the next keyword (“*”) card. Card 2 1 2 3 4 5 6 7 8 Variable B1BEG B1END B2BEG B2END B3BEG B3END B4BEG B4END Type I I I I I I I Part ID Range with Increment Cards. This Card 2 format applies to the LIST_GEN- ERATE_INCREMENT keyword option. For each block of parts add one card to the deck. This input ends at the next keyword (“*”) card. Card 2 1 2 3 4 5 6 7 8 Variable BBEG BEND INCR Type I I I VARIABLE DESCRIPTION SID DA1 DA2 DA3 DA4 Set ID. All part sets should have a unique set ID. First attribute default value, see remark 1 below. Second attribute default value Third attribute default value Fourth attribute default value SOLVER Name of solver using this set (MECH, CESE, etc.) PID PID1 PID2 ⋮ A1 A2 A3 A4 Part ID First part ID Second part ID ⋮ First part attribute, see remark 2 below. Second part attribute Third part attribute Fourth part attribute B[N]BEG First part ID in block N. B[N]END Last part ID in block N. All defined ID’s between and including B[N]BEG to B[N]END are added to the set. These sets are generated after all input is read so that gaps in the part numbering are not a problem. B[N]BEG and B[N]END may simply be limits on the ID’s and not part ID’s. VARIABLE DESCRIPTION First part ID in block. Last part ID in block. Part ID increment. Part IDs BBEG, BBEG+INCR, BBEG + 2 × INCR, and so on through BEND are added to the set. BBEG BEND INCR Remarks: 1. Part attributes can be assigned for some input types. For example, for airbags a time delay, DA1 = T1, can be defined before pressure begins to act along with a time delay, DA2 = T2, before full pressure is applied, (default T2 = T1), and for the constraint option, *CONSTRAINED_RIGID_BODY_STOPPERS one attrib- ute can be defined: DA1, the closure distance which activates the stopper con- straint. 2. The default part attributes can be overridden on the part cards; otherwise, A1 = DA1, etc. 3. This field is used by a non-mechanics solver to create a set defined on that solver’s mesh. By default, the set refers to the mechanics mesh. Purpose: Define a part set by combining part sets. *SET Card 1 1 2 3 4 5 6 7 8 Variable SID DA1 DA2 DA3 DA4 SOLVER Type I F F F F A Default none MECH Remark 1,2 1,2 1,2 1,2 3 Part Set Cards. Each card can be used to specify up to 8 part set IDs. Include as many cards of this kind as necessary. This input ends at the next keyword (“*”) card. Card 2… 1 2 3 4 5 6 7 8 Variable PSID1 PSID2 PSID3 PSID4 PSID5 PSID6 PSID7 PSID8 Type I I I I I I I I VARIABLE DESCRIPTION SID DA1 DA2 DA3 DA4 Set ID. All part sets should have a unique set ID. First attribute default value, see Remarks 1 and 2 below. Second attribute default value Third attribute default value Fourth attribute default value SOLVER Name of solver using this set (MECH, CESE, etc.) VARIABLE DESCRIPTION PSID[N] The Nth part set ID GT.0: PSIDn is added to SID, LT.0: all part sets with ID between PSID(i-1) and |PSIDi|, including PSID(i-1) and |PSIDi|, will be added to SID. PSID(i-1) has to be > 0 and has a magnitude smaller or equal to |PSIDi | when PSIDi < 0. Remarks: 1. Part attributes can be assigned for some input types. For example, for airbags a time delay, DA1 = T1, can be defined before pressure begins to act along with a time delay, DA2 = T2, before full pressure is applied, (default T2 = T1), and for the constraint option, *CONSTRAINED_RIGID_BODY_STOPPERS one attrib- ute can be defined: DA1, the closure distance which activates the stopper con- straint. 2. The default values for the part attributes are given in the contributing *SET_- PART_{OPTION} commands. Nonzero values of DA1, DA2, DA3, or DA4 in *SET_PART_ADD will override the respective default values. 3. This field is used by a non-mechanics solver to create a set defined on that solver’s mesh. By default, the set refers to the mechanics mesh. *SET_SEGMENT_{OPTION1}_{OPTION2} For OPTION1 the available options are: <BLANK> GENERAL For OPTION2 the available option is COLLECT Purpose: Define set of segments with optional identical or unique attributes. For three- dimensional geometries, a segment can be triangular or quadrilateral. For two- dimensional geometries, a segment is a line defined by two nodes and the GENERAL option does not apply. Card 1 1 2 3 4 5 6 7 8 Variable SID DA1 DA2 DA3 DA4 SOLVER Type I F Default none 0. Remarks 1 F 0. 1 F 0. 1 F A 0. MECH 1 4 Segment Cards. For each segment in the set include on card of this format. Set N3 = N4 for triangular segments. Include as many cards as necessary. This input ends at the next keyword (“*”) card. Card 2 Variable 1 N1 Type I 2 N2 I 3 N3 I Remarks 4 N4 I 2 5 A1 F 3 6 A2 F 3 7 A3 F 3 8 A4 F Generalized Part ID Range Cards. This Card 2 format applies to the GENERAL keyword option. Include as many cards as needed. This input ends at the next keyword (“*”) card. Card 2 1 Variable OPTION Type A 2 E1 I 3 E2 I 4 E3 5 E4 6 E5 7 E6 8 E7 I I or F I or F I or F I or F VARIABLE DESCRIPTION SID DA1 DA2 DA3 DA4 Set ID. All segment sets should have a unique set ID. First segment attribute default value, see remark 1 below. Second segment attribute default value Third segment attribute default value Fourth segment attribute default value SOLVER Name of solver using this set (MECH, CESE, etc.) N1 N2 N3 N4 A1 A2 A3 A4 NFLS SFLS Nodal point 𝑛1 Nodal point 𝑛2 Nodal point 𝑛3 Nodal point 𝑛4, see Remark 2 below. First segment attribute, see Remark 3 below. Second segment attribute Third segment attribute Fourth segment attribute Normal failure stress Shear failure stress. Failure criterion: OPTION Option for GENERAL. See table below. E1, …, E7 DESCRIPTION Specified entity. Each card must have an option specified. See table below. *SET The General Option: The “OPTION” column in the table below enumerates the allowed values for the “OPTION” variable in Card 2 for the GENERAL option. Likewise, the variables E1, …, E7 refer to the GENERAL option Card 2. Each of the following operations accept up to 7 arguments, but they may take fewer. Values of “En” left unspecified are ignored. OPTION DESCRIPTION ALL BOX BOX_SHELL BOX_SLDIO BOX_SOLID PART All exterior segments will be included in the set. Generate segments inside boxes having IDs E1, E2, and E3 with attributes having values E4, E5, E6, and E7. For shell elements one segment per shell is generated. For solid elements only those segments wrapping the solid part and pointing outward from the part will be generated. Generate segments inside boxes having IDs E1, E2, and E3 with attributes having values E4, E5, E6, and E7. The segments are only generated for shell elements. One segment per shell is generated. Generate segments inside boxes having IDs E1, E2, and E3 with attributes having values E4, E5, E6, and E7. Both exterior segments and inter-element segments are generated. Generate segments inside boxes having IDs E1, E2, and E3 with attributes having values E4, E5, E6, and E7. The segments are only generated for exterior solid elements Generate segments of parts E1, E2, and E3 with attributes E4, E5, E6, and E7. For shell elements one segment per shell is generated. For solid elements only those segments wrapping the solid part and pointing outward from the part will be generated. PART could refer to beam parts when defining 2D segments for traction application. DESCRIPTION *SET_SEGMENT PART_IO PSLDFi SEG VOL Generate segments from parts E1, E2, E3 with attributes E4, E5, E6, and E7. Same as the PART option above except that inter- element segments inside parts will be generated as well. This option is sometimes useful for single surface contact of solid elements to prevent negative volumes. Generate segments from the i’th face of solid parts E1, E2, E3 with attributes E4, E5, E6, and E7. See table below for face definition. Create segment with node IDs E1, E2, E3, and E4. Generate segments inside contact volume IDs E1, E2, and E3 with attributes having values E4, E5, E6, and E7. See BOX option for other details. VOL_SHELL Generate segments for shells inside contact volume IDs E1, E2, and E3 with attributes having values E4, E5, E6, and E7 VOL_SLDIO VOL_SOLID Generate segments for solid elements inside contact volume IDs E1, E2, and E3 with attributes E4, E5, E6, and E7. See BOX_- SLDIO for other details. Generate segments for solid elements inside contact volume IDs E1, E2, and E3 with attributes E4, E5, E6, and E7. See BOX_SOL- ID for other details. SET_SHELL Generate segments for shell elements in SET_SHELL_LIST with IDs E1, E2, and E3 with attributes E4, E5, E6, and E7. SET_SOLID SET_SLDIO SET_SLDFi Generate segments for solid elements in SET_SOLID_LIST with IDs E1, E2, and E3 with attributes E4, E5, E6, and E7. Generate segments for solid elements in SET_SOLID_LIST with IDs E1, E2, and E3 with attributes E4, E5, E6, and E7. Both exterior & interior segments are generated. Generate segments from the ith face of solid elements in SET_- SOLID_LIST with IDs E1, E2, and E3 with attributes E4, E5, E6, and E7. See table below for face definition. SET_TSHELL Generate segments for thick shell elements in SET_TSHELL_LIST with IDs of E1, E2, and E3 with attributes E4, E5, E6, and E7. Only exterior segments are generated. DESCRIPTION *SET SET_TSHIO Generate segments for thick shell elements in SET_TSHELL_LIST with IDs of E1, E2, and E3 with attributes E5, E5, E6, and E7. Both exterior & interior segments are generated. DBOX Segments inside boxes with IDs E1, …, E7 will be excluded. DBOX_SHELL Shell related segments inside boxes of IDs E1, …, E7 will be excluded. DBOX_SOLID Solid related segments inside boxes of IDs E1, …, E7 will be excluded. DPART Segments of parts with IDs E1, …, E7 will be excluded. DSEG DVOL Segment with node IDs E1, E2, E3, and E4 will be deleted. Segments inside contact volumes having IDs E1, …, E7 will be excluded. DVOL_SHELL Shell related segments inside contact volumes having IDs E1, …, E7 will be excluded. DVOL_SOLID Solid related segments inside contact volumes having IDs E1, …, E7 will be excluded. SALECPT Segments inside a box in Structured ALE mesh. E1 here is the S- ALE mesh ID (MSHID). E2, E3, E4, E5, E6, E7 correspond to XMIN, XMAX, YMIN, YMAX, ZMIN, ZMAX. They are the minimum and the maximum nodal indices along each direction in S-ALE mesh. This option is only to be used for Structured ALE mesh and should not be used in a mixed manner with other “_GENERAL” options. Please refer to *ALE_STRUCTURED_MESH_CONTROL_- POINTS and *ALE_STRUCTURED_MESH_CONTROL for more details. DESCRIPTION *SET_SEGMENT Segments on the face of Structured ALE mesh. E1 here is the S- ALE mesh ID (MSHID). E2, E3, E4, E5, E6, E7 correspond to -X, +X, -Y, +Y, -Z, +Z faces. Assigning 1 to these 6 values would include all the surface segments at these faces in the segment set. This option is only to be used for Structured ALE mesh and should not be used in a mixed manner with other “_GENERAL” options. Please refer to *ALE_STRUCTURED_MESH_CONTROL_- POINTS and *ALE_STRUCTURED_MESH_CONTROL for more details. SALEFAC Remarks: 1. Segment attributes can be assigned for some input types. For example, for the contact options. The attributes for the SLAVE surface are: DA1 (NFLS) = Normal failure stress, *CONTACT_TIEBREAK_SURFACE contact only, DA2 (SFLS) = Shear failure stress, *CONTACT_TIEBREAK_SURFACE contact only, DA3 (FSF) = Coulomb friction scale factor, DA4 (VSF) = Viscous friction scale factor, and the attributes for the MASTER surface are: DA3 (FSF) = Coulomb friction scale factor, DA4 (VSF) = Viscous friction scale factor. For airbags, see *AIRBAG, a time delay, DA1 = T1, can be defined before pres- sure begins to act on a segment along with a time delay, DA2 = T2, before full pressure is applied to the segment, (default T2 = T1), and for the constraint option, 2. To define a triangular segment make N4 equal to N3. 3. The default segment attributes can be overridden on these cards, otherwise, A1 = DA1, A2 = DA2, etc. 4. This field is used by a non-mechanics solver to create a set defined on that solver’s mesh. By default, the set refers to the mechanics mesh. FACE Hexahedron Pentahedron Tetrahedron 1 2 3 4 5 6 N1, N5, N8, N4 N2, N3, N7, N6 N1, N2, N6, N5 N4, N8, N7, N3 N1, N2, N5 N1, N2, N4 N4, N6, N3 N2, N3, N4 N1, N4, N3, N2 N1, N3, N2 N2, N3, N6, N5 N1, N4, N3 N1, N4, N3, N2 N1, N5, N6, N4 N5, N6, N7, N8 Table 4.1 Face definition of solid elements *SET_SEGMENT_ADD Purpose: Define a segment set by combining segment sets. Card 1 1 2 3 4 5 6 7 8 Variable SID SOLVER Type I A Default none MECH Remark 1 Segment Set Cards. Each card can be used to specify up to 8 segment set IDs. Include as many cards of this kind as necessary. This input ends at the next keyword (“*”) card. Card 2 1 2 3 4 5 6 7 8 Variable SSID1 SSID2 SSID3 SSID4 SSID5 SSID6 SSID7 SSID8 Type I I I I I I I I VARIABLE SID DESCRIPTION Set ID of new segment set. All segment sets should have a unique set ID. SOLVER Name of solver using this set (MECH, CESE, etc.) SSID[N] The Nth segment set ID on card2. Remarks: 1. This field is used by a non-mechanics solver to create a set defined on that solver’s mesh. By default, the set refers to the mechanics mesh. *SET Purpose: Define a segment set as the intersection, ∩, of a series of segment sets. The new segment set, SID, contains all segments common to the sets listed on all of the cards in format 2. Card 1 1 2 3 4 5 6 7 8 Variable SID SOLVER Type I A Default none MECH Remark 1 Segment Set Cards. For each SID in the intersection specify one field. Include as many cards as necessary. This input ends at the next keyword (“*”) card. Card 2 1 2 3 4 5 6 7 8 Variable SSID1 SSID2 SSID3 SSID4 SSID5 SSID6 SSID7 SSID8 Type I I I I I I I I VARIABLE SID DESCRIPTION Set ID of new segment set. All segment sets should have a unique set ID. SOLVER Name of solver using this set (MECH, CESE, etc.) SSID[N] The Nth segment set ID Remarks: 1. This field is used by a non-mechanics solver to create a set defined on that solver’s mesh. By default, the set refers to the mechanics mesh. *SET_2D_SEGMENT_{OPTION1}_{OPTION2} For OPTION1 the available options are: <BLANK> SET For OPTION2 the available option is: COLLECT Purpose: Define a set of boundary line segments in two-dimensional axisymmetric, plane stress, and plane strain geometries with optional attributes. This command does not apply to beam formulations 7 and 8. It is sometimes convenient for two- dimensional parts which are subject to adaptivity because the segments in the set are updated as the geometry adapts. Card Sets. For each set include a pair of cards 1 and 2. This input ends at the next keyword (“*”) card. Card 1 1 2 3 4 5 6 7 8 Variable SID DA1 DA2 DA3 DA4 F 0. 1 3 F 0. 1 4 F 0. 1 5 6 7 8 Type I F Default none 0. 1 2 Remarks Card 2 1 Variable PID/PSID Type Remarks I VARIABLE DESCRIPTION SID DA1 DA2 DA3 DA4 Set ID. All segment sets should have a unique set ID. First segment attribute default value, see remark 1 below. Second segment attribute default value Third segment attribute default value Fourth segment attribute default value PID/PSID Part ID or part set ID if SET option is specified. Remarks: 1. The boundary along r = 0 isn’t included in axisymmetric problems. 2. The common boundary between parts in the part set PSID is not included in the boundary segments. *SET_SHELL_{OPTION1}_{OPTION2} For OPTION1 the available options are: <BLANK> LIST COLUMN LIST_GENERATE LIST_GENERATE_INCREMENT GENERAL For OPTION2 the available option is: COLLECT The LIST_GENERATE and LIST_GENERATE_INCREMENT options will generate block(s) of shell element IDs between a starting ID and an ending ID. An arbitrary number of blocks can be specified to define the shell element set. Purpose: Define a set of shell elements with optional identical or unique attributes. Card 1 1 2 3 4 5 6 7 8 Variable SID DA1 DA2 DA3 DA4 Type I F Default none 0. Remarks 1 F 0. 1 F 0. 1 F 0. Shell Element ID Cards. This Card 2 format applies to LIST keyword option. Additionally, it applies to the case of an unset (<BLANK>) keyword option. Set one value per element in the set. Include as many cards as needed. This input ends at the next keyword (“*”) card. Card 2 1 2 3 4 5 6 7 8 Variable EID1 EID2 EID3 EID4 EID5 EID6 EID7 EID8 Type Remarks I 2 I 2 I 2 I 2 I 2 I 2 I 2 I 2 Shell Element ID with Column Cards. This Card 2 format applies to the COLUMN keyword option. Include one card per shell element in the set. Include as many cards as needed. This input ends at the next keyword (“*”) card. Card 2 1 Variable EID Type I Remarks 2 A1 F 3 3 A2 F 3 4 A3 F 3 5 A4 F 3 6 7 8 Shell Element ID Range Cards. This Card 2 format applies to the GENERATE keyword option. Set one pair of BNBEG and BNEND values per block of shell element IDs. Include as many cards as needed. This input ends at the next keyword (“*”) card. Card 2 1 2 3 4 5 6 7 8 Variable B1BEG B1END B2BEG B2END B3BEG B3END B4BEG B4END Type I I I I I I I Shell Element ID Range with Increment Cards. This Card 2 format applies to the LIST_GENERATE_INCREMENT keyword option. For each block of shell elements add one card to the deck. This input ends at the next keyword (“*”) card. Card 2 1 2 3 4 5 6 7 8 Variable BBEG BEND INCR Type I I I Generalized Shell Element ID Range Cards. This Card 2 format applies to the GENERAL keyword option. Include as many cards as needed. This input ends at the next keyword (“*”) card. Card 2 1 Variable OPTION Type A 2 E1 I 3 E2 I 4 E3 I 5 E4 I 6 E5 I 7 E6 I 8 E7 I VARIABLE DESCRIPTION SID DA1 DA2 DA3 DA4 EID1 EID2 ⋮ EID A1 A2 A3 Set ID. All shell sets should have a unique set ID. First attribute default value, see remark 1. Second attribute default value Third attribute default value Fourth attribute default value First shell element ID, see remark 2. Second shell element ID ⋮ Element ID First attribute Second attribute Third attribute DESCRIPTION A4 Fourth attribute BnBEG First shell ID in shell block n. *SET BnEND BBEG BEND INCR Last shell ID in block n. All defined ID’s between and including BnBEG to BnEND are added to the set. These sets are generated after all input is read so that gaps in the element numbering are not a problem. BnBEG and BnEND may simply be limits on the ID’s and not element IDs. First shell element ID in block. Last shell element ID in block. Shell element ID increment. Shell element IDs BBEG, BBEG + INCR, BBEG + 2 × INCR, and so on through BEND are added to the set. OPTION Option for GENERAL. See table below. E1, …, E7 Specified entity. Each card must have the option specified. See table below. The General Option: The “OPTION” column in the table below enumerates the allowed values for the “OPTION” variable in Card 2 for the GENERAL option. Likewise, the variables E1, …, E7 refer to the GENERAL option Card 2. Each of the following operations accept up to 7 arguments, but they may take fewer. Values of “En” left unspecified are ignored. OPTION ALL ELEM DESCRIPTION All shell elements will be included in the set. Shell elements E1, E2, E3, … will be included. DELEM Shell elements E1, E2, E3, … previously added will be excluded. PART Shell elements of parts E1, E2, E3, … will be included. DPART Shell elements of parts E1, E2, E3, … previously added will be excluded. BOX DBOX Remarks: *SET_SHELL DESCRIPTION Shell elements inside boxes E1, E2, E3, … will be included. Shell elements inside boxes E1, E2, E3, … previously added will be excluded. 1. Shell attributes can be assigned for some input types. For example, for contact options, the attributes for the SLAVE surface are: DA1 (NFLS) = Normal failure stress, *CONTACT_TIEBREAK_SURFACE contact only, DA2 (SFLS) = Shear failure stress, *CONTACT_TIEBREAK_SURFACE contact only, DA3 (FSF) = Coulomb friction scale factor, DA4 (VSF) = Viscous friction scale factor, and the attributes for the MASTER surface are: DA1 (FSF) = Coulomb friction scale factor, DA2 (VSF) = Viscous friction scale factor. 2. The default attributes are taken. 3. The default shell attributes can be overridden on these cards; otherwise, A1 = DA1, etc. Purpose: Define a shell set by combining shell sets. *SET Card 1 1 2 3 4 5 6 7 8 Variable SID Type I Default none Shell Element Set Cards. Each card can be used to specify up to 8 shell element set IDs. Include as many cards as necessary. This input ends at the next keyword (“*”) card. Card 2 1 2 3 4 5 6 7 8 Variable SSID1 SSID2 SSID3 SSID4 SSID5 SSID6 SSID7 SSID8 Type I I I I I I I I VARIABLE DESCRIPTION SID Set ID of new shell set. All shell sets should have a unique set ID. SSID[N] The Nth shell set ID on card2 *SET_SHELL_INTERSECT Purpose: Define a shell set as the intersection, ∩, of a series of shell sets. The new shell set, SID, contains all shells common to all sets on the cards of format 2. Card 1 1 2 3 4 5 6 7 8 Variable SID Type I Default none Shell Element Set Cards. For each shell element SID in the intersection input one field. Include as many cards as necessary. This input ends at the next keyword (“*”) card. Card 2 1 2 3 4 5 6 7 8 Variable SSID1 SSID2 SSID3 SSID4 SSID5 SSID6 SSID7 SSID8 Type I I I I I I I I VARIABLE DESCRIPTION SID Set ID of new shell set. All shell sets should have a unique set ID. SSID[N] The Nth shell set ID *SET_SOLID_{OPTION1}_{OPTION2} For OPTION1 the available options are: <BLANK> GENERATE GENERATE_INCREMENT GENERAL For OPTION2 the available option is: COLLECT The GENERATE and GENERATE_INCREMENT options will generate block(s) of solid element IDs between a starting ID and an ending ID. An arbitrary number of blocks can be specified to define the solid element set. Purpose: Define a set of solid elements. Card 1 1 2 3 4 5 6 7 8 Variable SID SOLVER Type I A Default none MECH Remark Solid Element ID Cards. This Card 2 format applies to the case of an unset (<BLANK>) keyword option. Set one value per solid element in the set. Include as many cards as needed. This input ends at the next keyword (“*”) card. Card 2 Variable 1 K1 Type I 2 K2 I 3 K3 I 4 K4 I 5 K5 I 6 K6 I 7 K7 I 8 K8 I Solid Element ID Range Cards. This Card 2 format applies to the GENERATE keyword option. Set one pair of BNBEG and BNEND values per block of solid elements. Include as many cards as needed. This input ends at the next keyword (“*”) card. Card 2 1 2 3 4 5 6 7 8 Variable B1BEG B1END B2BEG B2END B3BEG B3END B4BEG B4END Type I I I I I I I I Solid Element ID Range with Increment Cards. This Card 2 format applies to the GENERATE_INCREMENT keyword option. For each block of solid elements add one card to the deck. This input ends at the next keyword (“*”) card. Card 2 1 2 3 4 5 6 7 8 Variable BBEG BEND INCR Type I I Generalized Solid Element ID Range Cards. This Card 2 format applies to the GENERAL keyword option. Include as many cards as needed. This input ends at the next keyword (“*”) card. Card 2 1 Variable OPTION Type A 2 E1 I 3 E2 I 4 E3 I 5 E4 I 6 E5 I 7 E6 I 8 E7 I VARIABLE DESCRIPTION SID Set ID. All solid sets should have a unique set ID. SOLVER Name of solver using this set (MECH, CESE, etc.) K1 K2 ⋮ K8 First element ID Second element ID ⋮ Eighth element ID B[N]BEG First solid element ID in block N. B[N]END BBEG BEND INCR Last solid element ID in block N. All defined ID’s between and including B[N]BEG to B[N]END are added to the set. These sets are generated after all input is read so that gaps in the element numbering are not a problem. B[N]BEG and B[N]END may simply be limits on the ID’s and not element IDs. First solid element ID in block. Last solid element ID in block. Solid ID increment. Solid IDs BBEG, BBEG + INCR, BBEG + 2 × INCR, and so on through BEND are added to the set. OPTION Option for GENERAL. See table below. E1, ..., E7 Specified entity. Each card must have the option specified. See table below. *SET_SOLID The “OPTION” column in the table below enumerates the allowed values for the “OPTION” variable in Card 2 for the GENERAL option. Likewise, the variables E1, …, E7 refer to the GENERAL option Card 2. Each of the following operations accept up to 7 arguments, but they may take fewer. Values of “En” left unspecified are ignored. OPTION DESCRIPTION ALL All solid elements will be included in the set. ELEM Elements E1, E2, E3, ... will be included. DELEM Elements E1, E2, E3, ... previously added will be excluded. PART Elements of parts E1, E2, E3, ... will be included. DPART BOX DBOX SALECPT Elements of parts E1, E2, E3, ... previously added will be excluded. Elements inside boxes E1, E2, E3, ... will be included. Elements inside boxes E1, E2, E3, ... previously added will be excluded. Elements inside a box in Structured ALE mesh. E1 here is the S- ALE mesh ID (MSHID). E2, E3, E4, E5, E6, E7 correspond to XMIN, XMAX, YMIN, YMAX, ZMIN, ZMAX. They are the minimum and the maximum nodal indices along each direction in S-ALE mesh. This option is only to be used for Structured ALE mesh and should not be used in a mixed manner with other “_GENERAL” options. refer Please *ALE_STRUCTURED_MESH_CONTROL_- POINTS and *ALE_STRUCTURED_MESH_CONTROL for more details. to SALEFAC *SET DESCRIPTION Elements on the face of Structured ALE mesh. E1 here is the S- ALE mesh ID (MSHID). E2, E3, E4, E5, E6, E7 correspond to -X, +X, -Y, +Y, -Z, +Z faces. Assigning 1 to these 6 values would include all the boundary elements at these faces in the segment set. This option is only to be used for Structured ALE mesh and should not be used in a mixed manner with other “_GENERAL” options. refer *ALE_STRUCTURED_MESH_CONTROL_- Please POINTS and *ALE_STRUCTURED_MESH_CONTROL for more details. to Remarks: 1. This field is used by a non-mechanics solver to create a set defined on that solver’s mesh. By default, the set refers to the mechanics mesh. Purpose: Define a solid set by combining solid sets. *SET_SOLID_ADD Card 1 1 2 3 4 5 6 7 8 Variable SID SOLVER Type I A Default none MECH Remark 1 Node Set Cards. Each card can be used to specify up to 8 solid set IDs. Include as many cards as necessary. This input ends at the next keyword (“*”) card. Card 2 1 2 3 4 5 6 7 8 Variable SSID1 SSID2 SSID3 SSID4 SSID5 SSID6 SSID7 SSID8 Type I I I I I I I I VARIABLE DESCRIPTION SID Set ID of new solid set. All solid sets should have a unique set ID. SOLVER Name of solver using this set (MECH, CESE, etc.) SSID[N] The Nth solid set ID. Remarks: 1. This field is used by a non-mechanics solver to create a set defined on that solver’s mesh. By default, the set refers to the mechanics mesh. *SET Purpose: Define a solid set as the intersection, ∩, of a series of solid sets. The new solid set, SID, contains all common elements of all solid sets SSIDn. Card 1 1 2 3 4 5 6 7 8 Variable SID SOLVER Type I A Default none MECH Remark 1 Solid Element Set Cards. For each solid element SID in the intersection input one field. Include as many cards as necessary. This input ends at the next keyword (“*”) card. Card 2… 1 2 3 4 5 6 7 8 Variable SSID1 SSID2 SSID3 SSID4 SSID5 SSID6 SSID7 SSID8 Type I I I I I I I I VARIABLE DESCRIPTION SID Set ID of new solid set. All solid sets should have a unique set ID. SOLVER Name of solver using this set (MECH, CESE, etc.) SSIDN The Nth solid set ID on card2 Remarks: 1. This field is used by a non-mechanics solver to create a set defined on that solver’s mesh. By default, the set refers to the mechanics mesh. *SET_TSHELL_{OPTION1}_{OPTION2} For OPTION1 the available options are: <BLANK> GENERATE GENERAL For OPTION2 the available option is: COLLECT The option GENERATE will generate a block of thick shell element ID’s between a starting ID and an ending ID. An arbitrary number of blocks can be specified to define the set. Purpose: Define a set of thick shell elements. Card 1 1 2 3 4 5 6 7 8 Variable SID Type I Default none Thick Shell Element ID Cards. This Card 2 format applies to the case of an unset (<BLANK>) keyword option. Set one value per thick shell element in the set. Include as many cards as needed. This input ends at the next keyword (“*”) card. Card 2 Variable 1 K1 Type I 2 K2 I 3 K3 I 4 K4 I 5 K5 I 6 K6 I 7 K7 I 8 K8 Thick Shell Element ID Range Cards. This Card 2 format applies to the GENERATE keyword option. Set one pair of BNBEG and BNEND values per block of thick shell elements. Include as many cards as needed. This input ends at the next keyword (“*”) card. Card 2… 1 2 3 4 5 6 7 8 Variable B1BEG B1END B2BEG B2END B3BEG B3END B4BEG B4END Type I I I I I I I I Generalized Thick Shell Element ID Range Cards. This Card 2 format applies to the GENERAL keyword option. Include as many cards as needed. This input ends at the next keyword (“*”) card. Card 2… 1 Variable OPTION Type A 2 E1 I 3 E2 I 4 E3 I 5 E4 I 6 E5 I 7 E6 I 8 E7 I VARIABLE DESCRIPTION SID Set ID. All tshell sets should have a unique set ID. K1 K2 ⋮ K8 First thick shell element ID Second thick shell element ID ⋮ Eighth thick shell element ID B[N]BEG First thick shell element ID in block N. B[N]END Last thick shell element ID in block N. All defined ID’s between and including B[N]BEG to B[N]END are added to the set. These sets are generated after all input is read so that gaps in the element numbering are not a problem. B[N]BEG and B[N]END may simply be limits on the ID’s and not element IDs. OPTION Option for GENERAL. See table below. E1, ..., E7 *SET_TSHELL DESCRIPTION Specified entity. Each card must have the option specified. See table below. The General Option: The “OPTION” column in the table below enumerates the allowed values for the “OPTION” variable in Card 2 for the GENERAL option. Likewise, the variables E1, …, E7 refer to the GENERAL option Card 2. Each of the following operations accept up to 7 arguments, but they may take fewer. Values of “En” left unspecified are ignored. OPTION ALL ELEM DESCRIPTION All thick shell elements will be included in the set. Elements E1, E2, E3, ... will be included. DELEM Elements E1, E2, E3, ... previously added will be excluded. PART Elements of parts E1, E2, E3, ... will be included. DPART BOX DBOX Elements of parts E1, E2, E3, ... previously added will be excluded. Elements inside boxes E1, E2, E3, ... will be included. Elements inside boxes E1, E2, E3, ... previously added will be excluded. The keyword *TERMINATION provides an alternative way of stopping the calculation before the termination time is reached. The termination time is specified on the *CON- TROL_TERMINATION input and will terminate the calculation whether or not the options available in this section are active. Different types of termination may be defined: *TERMINATION_BODY Purpose: Terminate calculation based on rigid body displacements. For *TERMINA- TION_BODY the analysis terminates when the center of mass displacement of the rigid body specified reaches either the maximum or minimum value (stops 1, 2 or 3) or the displacement magnitude of the center of mass is exceeded (stop 4). If more than one condition is input, the analysis stops when any of the conditions is satisfied. Termination by other means than *TERMINATION input is controlled by the *CON- TROL_TERMINATION control card. Note that this type of termination is not active during dynamic relaxation. Part Cards. Add one card for each part having termination criterion. Include as many cards as necessary. This input terminates at the next keyword (“*”) card. Card 1 1 2 3 4 5 6 7 8 Variable PID STOP MAXC MINC Type I I Default none none F - F - VARIABLE DESCRIPTION PID STOP Part ID of rigid body, see *PART_OPTION. Stop criterion: EQ.1: global x direction, EQ.2: global y direction, EQ.3: global z direction, EQ.4: stop if displacement magnitude is exceeded. MAXC Maximum (most positive) displacement, options 1, 2, 3 and 4: EQ.0.0: MAXC set to 1.0e21. MINC Minimum (most negative) displacement, options 1, 2 and 3 above only: EQ.0.0: MINC set to -1.0e21. *TERMINATION Purpose: The analysis terminates when the magnitude of the contact interface resultant force is zero. If more than one contact condition is input, the analysis stops when any of the conditions is satisfied. Termination by other means than *TERMINATION input is controlled by the *CONTROL_TERMINATION control card. Note that this type of termination is not active during dynamic relaxation and does not apply to 2D contact types. Contact ID Cards. Add one card for contact ID having a termination criterion. Include as many cards as necessary. This input terminates at the next keyword (“*”) card. Card 1 1 2 3 4 5 6 7 8 Variable CID ACTIM DUR THRES DOF Type I F Default none none F - F 0.0 I 0 VARIABLE CID DESCRIPTION Contact ID. The contact ID is defined by the ordering of the contact input unless the TITLE option which allows the CID to be defined is used in the *CONTACT section. ACTIM Activation time. DUR THRES DOF Time duration of null resultant force prior to termination. This time is tracked only after the activation time is reached and the contact resultant forces are zero. EQ.0.0: Immediate termination after null force is detected. Any measured force magnitude below or equal to this specified threshold is taken as a null force. Default = 0.0 Option to consider only the force magnitude in the x, y, or z global directions corresponding to DOF = 1,2, and 3, respectively. *TERMINATION_CURVE Purpose: Terminate the calculation when the load curve value returns to zero. This termination can be used with the contact option *CONTACT_AUTO_MOVE. In this latter option, the load curve is modified to account for the movement of the master surface. Load Curve Card. For each load curve used as a termination criterion add a card. Include as many cards as necessary. This input ends at the next keyword (“*”) card. Card 1 1 2 3 4 5 6 7 8 Variable LCID ATIME Type I F Default none Remark 1 - VARIABLE DESCRIPTION LCID Load curve ID governing termination. ATIME Activation time. After this time the load curve is checked. If zero, see remark 1 below. Remarks: 1. If ATIME = 0.0, termination will occur after the load curve value becomes nonzero and then returns to zero. *TERMINATION_DELETED_SHELLS_{OPTION} Available options include: <BLANK> SET Purpose: Terminate the calculation when the number of deleted shells for a specified part ID exceeds the value defined here. This input has no effect for a part ID that is left undefined. Generally, this option should be used with the NFAIL1 and NFAIL4 parameters that are defined in the *CONTROL_SHELL control information. When using the SET option, termination will occur when NDS elements are deleted in any one of the parts in the part set PSID. Part (set) Cards. Include one card for each part having a termination criterion based on shell deletion. Include as many cards as necessary. This input ends at the next keyword (“*”) card. Card 1 1 2 3 4 5 6 7 8 Variable PID/PSID NDS Type I I Default none none VARIABLE DESCRIPTION PID / PSID Part ID or if option SET is active, part set ID. NDS Number of elements that must be deleted for the specified part ID’s, before an error termination occurs. *TERMINATION_DELETED_SOLIDS_{OPTION} Available options include: <BLANK> SET Purpose: Terminate the calculation when the number of deleted solids for a specified part ID exceeds the value defined here. This input has no effect for a part ID that is left undefined. When using the SET option, termination will occur when NDS elements are deleted in any one of the parts in the part set PSID. Part (set) Cards. Include one card for each part having a termination criterion based on solid element deletion. Include as many cards as necessary. This input ends at the next keyword (“*”) card. Card 1 1 2 3 4 5 6 7 8 Variable PID/PSID NDS Type I Default none I 1 VARIABLE DESCRIPTION PID/PSID Part ID or if option SET is active, part set ID. NDS Number of elements that must be deleted for the specified part ID’s, before an error termination occurs. *TERMINATION Purpose: Terminate calculation based on nodal point coordinates. The analysis terminates for *TERMINATION_NODE when the current position of the node specified reaches either the maximum or minimum value (stops 1, 2 or 3), or picks up force from any contact surface (stops 4). Termination by other means than *TERMINATION is controlled by the *CONTROL_TERMINATION control card. Note that this type of termination is not active during dynamic relaxation. Node Cards. Include one card for each node having a termination criterion. Include as many cards as desired. This input terminates at the next keyword (“*”) card. Card 1 1 2 3 4 5 6 7 8 Variable NID STOP MAXC MINC Type I I Default none none F - F - VARIABLE DESCRIPTION NID STOP MAXC MINC Node ID, see *NODE_OPTION. Stop criterion: EQ.1: global x direction, EQ.2: global y direction, EQ.3: global z direction, EQ.4: stop if node touches contact surface. Maximum (most positive) coordinate (options 1, 2 and 3) above only. Minimum (most negative) coordinate (options 1, 2 and 3) above only. *TERMINATION_SENSOR Purpose: Terminates the calculation when the switch condition defined in *SENSOR_- SWITCH is met. Switch ID Cards. Include one card for each switch controlling termination. Include as many cards as desired. This input ends at the next keyword (“*”) card. Card 1 1 2 3 4 5 6 7 8 Variable SWID Type I Default none VARIABLE SWID Remarks: DESCRIPTION ID of *SENSOR_SWITCH which will terminate the calculation when its condition is met. Only one *TERMINATION_SENSOR is allowed. If more than one *TERMINATION_SENSOR is defined; only the last one is effective. An example allowing more than one sensor_switch to terminate calculation: *SENSOR_DEFINE_ELEMENT $ Axial force of beam element 1 44,BEAM,1,AXIAL,FORCE *SENSOR_DEFINE_ELEMENT $ Axial force of beam element 2 55,BEAM,21,AXIAL,FORCE *SENSOR_SWITCH $a switch condition is met when the axial force of beam-1 >5.0 11,SENSOR,44,GT,5. *SENSOR_SWITCH $a switch condition is met when the axial force of beam-2 >10.0 22,SENSOR,55,GT,10. *SENSOR_SWITCH $ a switch condition is met when time >50. 33,TIME, , 50 *SENSOR_SWITCH_CALC-LOGIC $ a switch condition is met if both conditions $ of switch-11 and switch-33 are met, I.e., $ axial force of beam-1>5.0 and time>50 44,11,33 *SENSOR_SWITCH_CALC-LOGIC $ a switch condition is met if both conditions $ of switch-22 and switch-33 are met, I.e., $ axial force of beam-2>10.0 and time>50 55,33,22 *SENSOR_SWITCH_CALC-LOGIC $ a switch condition is met if the conditions $ of switch-44 or switch-55 is met, I.e., $ axial force of beam-1>5.0 and time>50 or $ axial force of beam-2>10.0 and time>50 66,44,-55 *TERMINATION_SENSOR $ job will be terminated when the switch condition of switch-66 is met, I.e., $ axial force of beam-1>5.0 and time>50 or $ axial force of beam-2>10.0 and time>50 66 *TITLE Purpose: Define job title. Card 1 1 2 3 4 5 6 7 8 Variable Type Default TITLE C LS-DYNA USER INPUT VARIABLE DESCRIPTION TITLE Heading to appear on output and in output files. *USER_INTERFACE_OPTION Available options include: CONTROL FRICTION FORCES CONDUCTIVITY Purpose: Define user defined input and allocate storage for user defined subroutines for the contact algorithms. See also *CONTROL_CONTACT. The CONTROL option above allows the user to take information from the contact interface for further action, e.g., stopping the analysis. A sample user subroutine is provided in Appendix F. or The FRICTION option may be used to modify the Coulomb friction coefficients in contact types 3, 5, or 10 (*CONTACT_SURFACE_TO_SURFACE, *CONTACT_- NODES_TO_SURFACE, *CONTACT_ONE_WAY_SURFACE_TO_SURFACE) according to contact information or to use a friction coefficient database. A sample user-defined friction subroutine is provided in Appendix G. For the subroutine to be called, the static friction coefficient FS on Card 2 of *CONTACT must be any nonzero value, and shell thickness offsets must be invoked in the contact by setting SHLTHK to 1 or 2 using *CONTROL_CONTACT or Opt. Card B in *CONTACT. The array length USRFRC in *CONTROL_CONTACT should be set to a value no less than the sum of the number of history variables NOC and the number of user-defined input parameters in *USER_INTERFACE_FRICTION. The CONDUCTIVITY option is used to define heat transfer contact conductance properties for thermal contacts. Card 1 1 2 3 4 5 6 7 8 Variable IFID NOC NOCI NHSV Type I I I I Default none none none Card 2 1 2 3 4 5 6 7 8 Variable UC1 UC2 UC3 UC4 UC5 UC6 UC7 UC8 Type F F F F F F F F VARIABLE DESCRIPTION IFID NOC NOCI NHSV UC1 UC2 ⋮ Interface number Number of history variables for interface. The number should not exceed the length of the array defined on *CONTROL_CON- TACT. See Remarks. Initialize the first NOCI history variables in the input. NOCI must be smaller or equal to NOC. Number of history variables per interface node (only for friction and conductivity interface). First user defined input parameter. Second user defined input parameter. ⋮ UC[N] Last user defined input parameter, where N = NOCI. The FORCES option is used to collect contact nodal forces from specified contact ID list for user subroutines. Card 1 1 2 3 4 5 6 7 8 Variable NCONT Type I Default none Card 2 1 2 3 4 5 6 7 8 Variable CID1 CID2 CID3 CID4 CID5 CID6 CID7 CID8 Type I I I I I I I I VARIABLE DESCRIPTION IFID Interface number NCONT Number of contact ID. If NCONT LE. 0, all contacts will be used. CID1 CID2 ⋮ First contact user ID. Second contact user ID. ⋮ CID[N] Last contact user ID, where N = NCONT. Remarks: The (NOC) interface variables (of which NOCI are initialized) are passed as arguments to the user defined subroutine. See Appendix G for the full list of arguments passed to the subroutine. This keyword is not supported by segment based contact which is invoked by setting SOFT = 2 on optional card A of the *CONTACT card. *USER_LOADING Purpose: Provide a means of applying pressure and force boundary conditions. The keyword *USER_LOADING activates this option. Input here is optional with the input being read until the next “*” keyword appears. The data read here is to be stored in a common block provided in the user subroutine, LOADUD. This data is stored and retrieved from the restart files. Parameter Cards. Add one card for each input parameter. Include as many cards as needed. This input ends at the next keyword (“*”) card. Card 1… 1 2 3 4 5 6 7 8 Variable PARM1 PARM2 PARM3 PARM4 PARM5 PARM6 PARM7 PARM8 Type F F F F F F F F Default none none none none none none none none VARIABLE DESCRIPTION PARM[N] This is the Nth user input parameter. *USER Purpose: Provides a means to apply user-defined loading to a set of nodes or segments. Loading could be nodal force, body force, temperature distribution, and pressure on segment or beam. Set Cards. Add a card for each set to which a load is applied. Include as many cards as necessary. This input ends at the next keyword (“*”) card. Card 1 1 2 3 4 5 6 7 8 Variable SID LTYPE LCID CID SF1 SF2 SF3 IDULS Type I A I I F F F I Default none none none global none none none Seq. # VARIABLE SID DESCRIPTION ID of the set to which user-defined loading will be applied. Set type depends on the type of loading, see LTYPE. LTYPE Loading type: EQ.“FORCEN”: Force a will be applied to node set SID. The load is to be given in units of force. EQ.“BODYFN”: Body force density will be applied to node set SID. The load is to be given in units of force per volume. EQ.“TEMPTN”: Temperature will be assigned to node set SID. This option cannot be coexist with *LOAD_- THERMAL_VARIABLE. In other word, users can only use either this option or *LOAD_- THERMAL_VARIABLE to specify temperature distribution, not both of them, EQ.“PRESSS”: Pressure will be applied to segment set SID. The load is to be given in units of force per ar- ea. EQ.“PRESSB”: Pressure in units of force per length will be applied to beam set SID. LCID CID *USER_LOADING_SET DESCRIPTION Load curve, a function of time. Its current value, crv, is passed to user subroutine LOADSETUD. Optional coordinate system along which scale factors SFi is defined. Global system is the default system. SF[i] Scale factor of loading magnitude, when LTYPE LTYPE.EQ.“FORCEN”: SFi is the factor along 𝑖th direction of CID. For example, set SF1 = 1. and the others to zero if the load is to be ap- plied in the positive 𝑥-direction. This applies whether the global or a local coordinate system is used. LTYPE.EQ.“BODYFN”: See “EQ.FORCEN” LTYPE.EQ.“PRESSS”: SF1 is used as the scale factor, SF2 and SF3 are ignored, LTYPE.EQ.“PRESSB”: Scale factor along 𝑟, 𝑠, 𝑡 axis of beam. Each USER_LOADING_SET can be assigned a unique ID, which is passed to user subroutine LOADSETUD and allows multiple loading definitions by using a single user subroutine, LOADSE- TUD. If no value is input, LS-DYNA will assign a sequence number to each USER_LOADING_SET based on its definition sequence. IDULS Remarks: *USER_LOADING_SET activates the loading defined in user subroutine LOADSETUD, part of dyn21.F. When both *USER_LOADING_SET and *USER_LOADING are defined, *USER_LOADING is only used to define user-defined parameters, PARMn; not to activate user subroutine LOADUD. Therefore only loading defined in LOADSETUD will be applied. More than one loading definitions can be defined and assigned a unique ID, that enables multiple loading to be taken care of by a single subroutine, LOADSETUD, as shown below: subroutine loadsetud(time,lft,llt,crv,iduls,parm) c c Input (not modifiable) c x : coordinate of node or element center c d : displacement of node or element center c v : velocity of node or element center c temp: temperature of node or element center c crv : value of LCID at current time c isuls : id of user_loading_set c parm: parameters defined in *USER_LOADING c Output (defined by user) c udl : user-defined load value include 'nlqparm' C_TASKCOMMON (aux8loc) common/aux8loc/ & x1(nlq),x2(nlq),x3(nlq),v1(nlq),v2(nlq),v3(nlq), & d1(nlq),d2(nlq),d3(nlq),temp(nlq),udl(nlq),tmp(nlq,12) c c sample code c if (iduls.eq.100) then c do i=lft,llt c your code here c udl(i)=.......... c enddo c elseif (iduls.eq.200) then c do i=lft,llt c udl(i)=.......... c enddo c endif return end Restart Input Data Restart Input Data In general three categories of restart actions are possible with LS-DYNA and are outlined in the following discussion: 1. A simple restart occurs when LS-DYNA was interactively stopped before reaching the termination time. Then, by specifying the R=rtf command line option on the execution line, LS-DYNA restarts the calculation from the termi- nation point. The calculation will pick up at the specified termination time. see INTRODUCTION, Execution Syntax. No additional input deck is required. 2. For small modifications of the restart run LS-DYNA offer a “small restart” capability which can a) reset termination time, b) reset output printing interval, c) reset output plotting interval, d) delete contact surfaces, e) delete elements and parts, f) switch deformable bodies to rigid, g) switch rigid bodies to deformable, h) change damping options. All modifications to the problem made with the restart input deck will be re- flected in subsequent restart dumps. All the members of the file families are consecutively numbered beginning from the last member prior to termination. For a small restart run a small input deck replaces the standard input deck on the execution line which must have at least the following command line arguments: LS-DYNA I=restartinput R=D3DUMPnn where D3DUMPnn (or whatever name is chosen for the family member) is the nth restart file from the last run where the data is taken. LS-DYNA automati- cally detects that a small input deck is used since the I=restartinput file may contain only the restart keywords (excluding *STRESS_INITIALIZATION): *CHANGE_OPTION *CONTROL_SHELL *CONTROL_TERMINATION *CONTROL_TIMESTEP *DAMPING_GLOBAL *DATABASE_OPTION *DATABASE_BINARY_OPTION *DELETE_OPTION *INTERFACE_SPRINGBACK_LSDYNA *RIGID_DEFORMABLE_OPTION *STRESS_INITIALIZATION_{OPTION} *TERMINATION_OPTION *TITLE *KEYWORD *CONTROL_CPU *DEFINE_OPTION *SET_OPTION The user has to take care that nonphysical modifications to the input deck are avoided; otherwise, complete nonsense may be the result. 3. If many modifications are desired a full restart may be the appropriate choice. A full restart is selected by including a full model along with a *STRESS_INITIAL- IZATION keyword card and possibly other restart cards. As mentioned in the Restart Analysis subsection of the Introduction portion of the manual, either all parts or some subset of parts can be made for the stress initialization. Remarks: a) In a full restart, only those nodes and elements defined in the full restart deck will be present in the analysis after the full restart is initiated. But as a convenience, any of those nodes or elements can be deleted using the *DELETE command. Restart Input Data b) In a small restart, velocities of nodes come from the dump file by default but those velocities can be changed using *CHANGE_VELOCITY_.... c) In a full restart, velocities of pre-existing nodes come from the dump file by default but those velocities can be changed using *CHANGE_VELOCI- TY_.... To set the starting velocities for new nodes in a full restart, use *INITIAL_VELOCITY_.... d) Pre-existing contacts, in general, carry forward seamlessly using data from the d3dump (or d3full if MPP) database. It is important that the contact ID(s) in the full restart input deck match the contact ID(s) in the original input deck if the intent is for the contacts to be initialized using data from the d3dump/d3full database. EXCEPTION: In the special case of MPP, a *CONTACT_AUTOMATIC_GENERAL contact in the full restart input deck is treated as a brand new contact and is not initialized using data from d3full. e) Only sets utilizing element IDs and node IDs are permitted in a small re- start deck; part IDs are not recognized. Sets referenced by other com- mands in a small restart deck must be defined in the small restart deck. *CHANGE_OPTION Purpose: Change solution options. Available options include: BOUNDARY_CONDITION CONTACT_SMALL_PENETRATION CURVE_DEFINITION OUTPUT RIGIDWALL_GEOMETRIC RIGIDWALL_PLANAR RIGID_BODY_CONSTRAINT RIGID_BODY_INERTIA RIGID_BODY_STOPPER STATUS_REPORT_FREQUENCY THERMAL_PARAMETERS VELOCITY VELOCITY_GENERATION VELOCITY_NODE VELOCITY_RIGID_BODY VELOCITY_ZERO Boundary Condition Cards. This card 1 format is for the BOUNDARY_CONDITION keyword option. Add one card for each boundary condition. This card imposes additional boundary conditions. It does not remove previously imposed conditions (for example, this option will not free a fixed node). This input ends at the next keyword (“*”) card. Card 1 1 2 3 4 5 6 7 8 Variable NID BCC Type I I VARIABLE DESCRIPTION NID BCC Nodal point ID, see also *NODE. New translational boundary condition code: EQ.1: constrained 𝑥 displacement, EQ.2: constrained 𝑦 displacement, EQ.3: constrained 𝑧 displacement, EQ.4: constrained 𝑥 and 𝑦 displacements, EQ.5: constrained 𝑦 and 𝑧 displacements, EQ.6: constrained 𝑧 and 𝑥 displacements, EQ.7: constrained 𝑥, 𝑦, and 𝑧 displacements. Small Penetration Check Cards. This Card 1 format is for the CONTACT_SMALL_ PENETRATION keyword option. Set one value for each contact surface ID where the small penetration check is to be turned on. The input terminates at the next keyword (“*”) card. See the PENCHK variable in *CONTACT. Card 1 1 Variable ID1 2 ID2 3 ID3 4 ID4 5 ID5 6 ID6 7 ID7 8 ID8 Type I I I I I I I I VARIABLE DESCRIPTION IDn Contact ID for surface number n. Load Curve Redefinition Cards. This Card 1 format is for the CURVE_DEFINITION keyword option. The new load curve must contain the same number of points as the curve it replaces. The curve should be defined according to the DEFINE_CURVE section of the manual. This input terminates when the next “*” card is encountered. Offsets and scale factors are ignored. Card 1 1 2 3 4 5 6 7 8 Variable LCID Type I VARIABLE DESCRIPTION LCID Load curve ID ASCII Output Overwrite Card. This format applies to the OUTPUT keyword option. Card 1 1 2 3 4 5 6 7 8 Variable IASCII Type I VARIABLE IASCII DESCRIPTION Flag to control manner of outputing ASCII data requested by *DATABASE_OPTION commands in a full restart deck: EQ.0: Full restart overwrites existing ASCII output (default), EQ.1: Full restart appends to existing ASCII output. Rigidwall modification. The format for the RIGIDWALL_GEOMETRIC and RIGIDWALL_PLANAR cards is identical to the original cards , however there are restrictions on the entries that may be changed: only those entries that define the size and orientation of the rigid walls may be changed, but not any of the others (e.g., the type). Rigid Body Constraint Modification Cards. This format for Card 1 applies to the RIGID_BODY_CONSTRAINT keyword option. This option can change translation and rotational boundary condition on a rigid body. This input ends at the next keyword (“*”) card. See CONSTRAINTED_RIGID_BODIES. 1 Variable PID Type I 2 TC I 3 RC I *RESTART INPUT DATA 4 5 6 7 8 VARIABLE DESCRIPTION PID TC Part ID, see *PART. Translational constraint: EQ.0: no constraints, EQ.1: constrained 𝑥 displacement, EQ.2: constrained 𝑦 displacement, EQ.3: constrained 𝑧 displacement, EQ.4: constrained 𝑥 and 𝑦 displacements, EQ.5: constrained 𝑦 and 𝑧 displacements, EQ.6: constrained 𝑧 and 𝑥 displacements, EQ.7: constrained 𝑥, 𝑦, and 𝑧 displacements. RC Rotational constraint: EQ.0: no constraints, EQ.1: constrained 𝑥 rotation, EQ.2: constrained 𝑦 rotation, EQ.3: constrained 𝑧 rotation, EQ.4: constrained 𝑥 and 𝑦 rotations, EQ.5: constrained 𝑦 and 𝑧 rotations, EQ.6: constrained 𝑧 and 𝑥 rotations, EQ.7: constrained 𝑥, 𝑦, and 𝑧 rotations. Card sets for RIGID_BODY_INERTIA keyword option. This option supports changing the mass and inertia properties of a rigid body. Include as many pairs of the following two cards as necessary. This input ends at the next keyword (“*”) card. The inertia tensor is specified relative to the coordinate system set in *MAT_RIGID at the start of the calculation, which is fixed in the rigid body and tracks the rigid body rotation. Card 1 Variable 1 ID 2 PID 3 TM Type I I F 4 5 6 7 8 Card 2 1 Variable IXX 2 IXY 3 IXZ 4 IYY 5 IYZ 6 IZZ 7 8 Type F F F F F F VARIABLE DESCRIPTION ID PID TM IXX IXY IXZ IYY IYZ IZZ ID for this change inertia input. Part ID, see *PART. Translational mass. 𝐼𝑥𝑥, 𝑥𝑥 component of inertia tensor. 𝐼𝑥𝑦 𝐼𝑥𝑧 𝐼𝑦𝑦 𝐼𝑦𝑧 𝐼𝑧𝑧 Card sets for the RIGID_BODY_STOPPERS keyword option. This option is for redefining existing stoppers. Include as many pairs of cards as necessary. This input terminates when the next “*” card is encountered. See *CONSTRAINED_RIGID_- BODY_STOPPERS. Note that new stopper definitions cannot be introduced in this section. Existing stoppers can be modified. Card 1 1 2 3 4 5 6 7 Variable PID LCMAX LCMIN PSIDMX PSIDMN LCVMNX DIR 8 VID I 0 3 I 0 4 I 0 5 I I I 0 required 0 6 7 8 Type I I Default required 0 Card 2 1 2 Variable BIRTH DEATH Type Default F 0 F 1028 VARIABLE DESCRIPTION PID Part ID of master rigid body, see *PART. LCMAX Load curve ID defining the maximum coordinate as a function of time: EQ.0: no limitation of the maximum displacement. New curves can be defined by the *DEFINE_CURVE within the present restart deck. (Not applicable for small deck restart). LCMIN Load curve ID defining the minimum coordinate as a function of time: EQ.0: no limitation of the minimum displacement. New curves can be defined by the *DEFINE_CURVE within the pre- sent restart deck. (Not applicable for small deck restart). PSIDMX Optional part set ID of rigid bodies that are slaved in the maximum coordinate direction to the master rigid body. This option requires additional input by the *SET_PART definition. VARIABLE PSIDMN DESCRIPTION Optional part set ID of rigid bodies that are slaved in the minimum coordinate direction to the master rigid body. This option requires additional input by the *SET_PART definition. LCVMNX Load curve ID which defines the maximum absolute value of the velocity that is allowed within the stopper: EQ.0: no limitation of the minimum displacement. DIR Direction stopper acts in: EQ.1: 𝑥-translation, EQ.2: 𝑦-translation, EQ.3: 𝑧-translation, EQ.4: arbitrary, defined by vector VID, EQ.5: 𝑥-axis rotation, EQ.6: 𝑦-axis rotation, EQ.7: 𝑧-axis rotation, EQ.8: arbitrary, defined by vector VID. VID Vector for arbitrary orientation of stopper. The vector must be defined by a *DEFINE_VECTOR within the present restart deck. BIRTH Time at which stopper is activated. DEATH Time at which stopper is deactivated. Remarks: The optional definition of part sets in minimum or maximum coordinate directions allows the motion to be controlled in an arbitrary direction. D3HSP Interval Change Card. This card format applies to the STATUS_REPORT_ FREQUENCY keyword option. Card 1 1 2 3 4 5 6 7 8 Variable IKEDIT Type VARIABLE DESCRIPTION IKEDIT Problem status report interval steps in the D3HSP output file: EQ.0: interval remains unchanged. Card set for the THERMAL_PARAMETERS keyword option. This option is for changing the parameters used by a thermal or coupled structural/thermal analysis. See *CONTROL_THERMAL. Add the two following cards to the deck (they do not repeat). 3 4 5 6 7 8 TMIN TMAX DTEMP TSCP F 3 F 4 F 5 F 6 7 8 Card 1 Variable 1 TS Type I Card 2 1 2 DT F 2 Variable REFMAX TOL Type I F VARIABLE DESCRIPTION TS Thermal time step code: EQ.0: No change, EQ.1: Fixed time step, EQ.2: variable time step. DT Thermal time step on restart: EQ.0: No change. TMIN Minimum thermal time step: EQ.0: No change. TMAX Maximum thermal time step: EQ.0: No change. VARIABLE DESCRIPTION DTEMP Maximum temperature change in a thermal time step: EQ.0: No change. TSCP Time step control parameter (0.0 < TSCP < 1.0 ): EQ.0: No change. REFMAX Maximum number of reformations per thermal time step: EQ.0: No change. TOL Non-linear convergence tolerance: EQ.0: No change. Node Set Velocity Card Sets. The formats for Cards 1 and 2 apply to the VELOCITY and VELOCITY_ONLY keyword options. These options are for setting velocity fields on node sets at restart. For each node set add one pair of the following cards. This input ends at the next keyword (“*”) card. Undefined nodes (not listed on a set velocity card) will have their nodal velocities reset to zero if a *CHANGE_VELOCITY definition is encountered in the restart deck. However, if any of the *CHANGE_VELOCITY definitions have ONLY appended, then only the specified nodes will have their nodal velocities modified. Card 1 1 2 3 4 5 6 7 8 Variable NSID Type I Default none Remark Variable 1 VX Type F Default 0. 2 VY F 0. 3 VZ F 0. *RESTART INPUT DATA 4 5 6 7 8 VXR VYR VZR F 0. F 0. F 0. VARIABLE DESCRIPTION NSID Nodal set ID containing nodes for initial velocity. Velocity in 𝑥-direction. Velocity in 𝑦-direction. Velocity in 𝑧-direction. Rotational velocity about the 𝑥-axis. Rotational velocity about the 𝑦-axis. Rotational velocity about the 𝑧-axis. VX VY VZ VXR VYR VZR Remarks: 1. If a node is initialized on more than one input card set, then the last set input will determine its velocity, unless it is specified on a *CHANGE_VELOCITY_- NODE card. 2. Undefined nodes will have their nodal velocities set to zero if a *CHANGE_VE- LOCITY definition is encountered in the restart deck. 3. If both *CHANGE_VELOCITY and *CHANGE_VELOCITY_ZERO cards are defined then all velocities will be reset to zero. Velocity generation cards. The velocity generation cards for the VELOCITY_ GENERATION option are identical to the standard velocity generation cards , and all parameters may be changed. Nodal Point Velocity Cards. This format applies to the VELOCITY_NODE and VELOCITY_NODE_ONLY keyword options. These option support changing nodal velocities. This input ends at the next keyword (“*”) card. Card 1 1 Variable NID Type I 2 VX F Default none 0. 3 VY F 0. 4 VZ F 0. 5 6 7 8 VXR VYR VZR F 0. F 0. F 0. VARIABLE DESCRIPTION NID Node ID Translational velocity in 𝑥-direction. Translational velocity in 𝑦-direction. Translational velocity in 𝑧-direction. Rotational velocity about the 𝑥-axis. Rotational velocity about the 𝑦-axis. Rotational velocity about the 𝑧-axis. VX VY VZ VXR VYR VZR Remarks: 1. Undefined nodes (not listed on a point velocity card) will have their nodal velocities reset to zero if a *CHANGE_VELOCITY_NODE definition is encoun- tered in the restart deck. However, if any of the *CHANGE_VELOCITY or CHANGE_VELOCITY_NODE definitions have_ONLY appended, then only the specified nodes will have their nodal velocities modified. 2. 3. If a node is initialized on more than one input card set, then the last set input will determine its velocity, unless it is specified on a *CHANGE_VELOCITY_- NODE card. If both *CHANGE_VELOCITY and *CHANGE_VELOCITY_ZERO cards are defined then all velocities will be reset to zero. Rigid Body Velocity Cards. This Card 1 format applies to the VELOCITY_RIGID_ BODY keyword option. This option allows for setting the velocity components of a rigid body at restart. Include as many of these cards as desired. This input ends at the next keyword (“*”) card. Card 1 1 Variable PID Type I 2 VX F Default none 0. 3 VY F 0. 4 VZ F 0. 5 6 7 8 VXR VYR VZR F 0. F 0. F 0. VARIABLE DESCRIPTION Part ID of rigid body. Translational velocity in 𝑥-direction. Translational velocity in 𝑦-direction. Translational velocity in 𝑧-direction. Rotational velocity about the 𝑥-axis. Rotational velocity about the 𝑦-axis. Rotational velocity about the 𝑧-axis. PID VX VY VZ VXR VYR VZR Remarks: 1. Rotational velocities are defined about the center of mass of the rigid body. 2. Rigid bodies not defined in this section will not have their velocities modified. Restarting the Model at Rest. The VELOCITY_ZERO option resets the velocities to zero at the start of the restart. There are no data cards associated with *CHANGE_VE- LOCITY_ZERO. *CONTROL_DYNAMIC_RELAXATION Purpose: Define controls for dynamic relaxation. Card 1 1 2 3 4 5 6 7 8 Variable NRCYCK DRTOL DRFCTR DRTERM TSSFDR IRELAL EDTTL IDRFLG Type I F F F F Default 250 0.001 0.995 ∞ TSSFAC Remarks 1 1 1 1 1 I 0 F 0.0 I 0 1 VARIABLE NRCYCK DESCRIPTION Number of iterations between convergence checks, for dynamic relaxation option (default = 250). DRTOL Convergence (default = 0.001). tolerance for dynamic relaxation option DRFCTR Dynamic relaxation factor (default = .995). DRTERM TSSFDR IRELAL EDTTL Optional termination time for dynamic relaxation. Termination occurs at this time or when convergence is attained (de- fault = infinity). Scale factor for computed time step during dynamic relaxation. If zero, the value is set to TSSFAC defined on *CONTROL_TERMI- NATION. After converging, the scale factor is reset to TSSFAC. Automatic control for dynamic relaxation option based on algorithm of Papadrakakis [1981]. Convergence relaxation. tolerance on automatic control of dynamic IDRFLG Dynamic relaxation flag for stress initialization: EQ.0: not active, EQ.1: dynamic relaxation is activated. Remarks: 1. 2. If a dynamic relaxation relaxation analysis is being restarted at a point before convergence was obtained, then NRCYCK, DRTOL, DRFCTR, DRTERM and TSSFDR will default to their previous values, and IDRFLG will be set to 1. If dynamic relaxation is activated after a restart from a normal transient analysis LS-DYNA continues the output of data as it would without the dynam- ic relaxation being active. This is unlike the dynamic relaxation phase at the beginning of the calculation when a separate database is not used. Only load curves that are flagged for dynamic relaxation are applied after restarting. *CONTROL_SHELL Purpose: Change failure parameters NFAIL1 and NFAIL4 if necessary. These parameters must be nonzero in the initial run. Card 1 1 2 3 4 5 6 7 8 Variable Type Card 2 1 2 3 4 5 6 7 8 Variable Type VARIABLE NFAIL1 NFAIL1 NFAIL4 PSNFAIL I I I DESCRIPTION Flag to check for highly distorted under-integrated shell elements, print a message, and delete the element or terminate. Generally, this flag is not needed for one point elements that do not use the warping stiffness. A distorted element is one where a negative jacobian exists within the domain of the shell, not just at The checks are made away from the integration points. integration points to enable the bad elements to be deleted before an instability leading to an error termination occurs. This test will increase CPU requirements for one point elements. EQ.1: print message and delete element. EQ.2: print message, write d3dump file, and terminate GT.2: print message and delete element. When NFAIL1 elements are deleted then write D3dump file and termi- nate. These NFAIL1 failed elements also include all shell elements that failed for other reasons than distortion. Before the d3dump file is written, NFAIL1 is doubled, so the run can immediately be continued if desired. VARIABLE NFAIL4 DESCRIPTION Flag to check for highly distorted fully-integrated shell elements, print a message, and delete the element or terminate. Generally, this flag is recommended. A distorted element is one where a negative jacobian exists within the domain of the shell, not just at integration points. The checks are made away from the integration points to enable the bad elements to be deleted before an instability leading to an error termination occurs. EQ.1: print message and delete element. EQ.2: print message, write d3dump file, and terminate GT.2: print message and delete element. When NFAIL4 elements are deleted then write d3dump file and termi- nate. These NFAIL4 failed elements also include all shell elements that failed for other reasons than distortion. Before the d3dump file is written, NFAIL4 is doubled, so the run can immediately be continued if desired. PSNFAIL Optional shell part set ID specifying which part IDs are checked by the NFAIL1, NFAIL4, and W-MODE options. If zero, all shell part IDs are included. *CONTROL_TERMINATION Purpose: Stop the job. Card 1 2 3 4 5 6 7 8 Variable ENDTIM ENDCYC Type F I VARIABLE DESCRIPTION ENDTIM Termination time: EQ.0.0: Termination time remains unchanged. ENDCYC Termination cycle. The termination cycle is optional and will be used if the specified cycle is reached before the termination time. EQ.0.0: Termination cycle remains unchanged. Remarks: This is a reduced version of the *CONTROL_TERMINATION card used in the initial input deck. RESTART INPUT DATA Purpose: Set time step size control using different options. Card 1 2 3 4 5 6 7 8 Variable DUMMY tssfac ISDO DUMMY DT2MS LCTM Type F F I F F I VARIABLE DESCRIPTION DUMMY Dummy field, see remark 1 below. TSSFAC Scale factor for computed time step. EQ.0.0: TSSFAC remains unchanged. ISDO Basis of time size calculation for 4-node shell elements, ISDO 3- node shells use the shortest altitude for options 0,1 and the shortest side for option 2. This option has no relevance to solid elements, which use a length based on the element volume divided by the largest surface area: EQ.0: characteristic length = area/(longest side), EQ.1: characteristic length = area/(longest diagonal), EQ.2: based on bar wave speed and MAX [shortest side, area/longest side]. THIS LAST OPTION CAN GIVE A MUCH LARGER TIME STEP SIZE THAT CAN LEAD TO INSTABILITIES IN SOME APPLICATIONS, ESPE- CIALLY WHEN TRIANGULAR ELEMENTS ARE USED. DUMMY Dummy field, see remark 1 below. DT2MS New time step for mass scaled calculations. Mass scaling must be active in the time zero analysis. EQ.0.0: DT2MS remains unchanged. LCTM Load curve ID that limits maximum time step size: EQ.0: LCTM remains unchanged. Remarks: 1. This a reduced version of the *CONTROL_TIMESTEP used in the initial analysis. The dummy fields are included to maintain compatibility. If using free format input then a 0.0 should be entered for the dummy values. RESTART INPUT DATA Purpose: Define mass weighted nodal damping that applies globally to the deformable nodes. Card 1 2 3 4 5 6 7 8 Variable LCID VALDMP Type Default I 0 F 0.0 VARIABLE DESCRIPTION LCID Load curve ID which specifies node system damping: EQ.n: system damping is given by load curve n. The damping force applied to each node is f = -d(t) mv, where d(t) is defined by load curve n. VALDMP System damping constant, d (this option is bypassed if the load curve number defined above is nonzero). *DATABASE_OPTION Options for ASCII files include. If a file is not specified in the restart deck then the output interval for the file will remain unchanged. SECFORC Cross section forces. RWFORC Wall forces. NODOUT Nodal point data. ELOUT Element data. GLSTAT Global data. DEFORC Discrete elements. MATSUM Material energies. NCFORC Nodal interface forces. RCFORC Resultant interface forces. DEFGEO Deformed geometry file SPCFORC Set dt for spc reaction forces. SWFORC Nodal constraint reaction forces (spot welds and rivets). ABSTAT Set dt for airbag statistics. NODFOR Set dt for nodal force groups. BNDOUT Boundary condition forces and energy RBDOUT Set dt for rigid body data. GCEOUT Set dt for geometric contact entities. SLEOUT Set dt for sliding interface energy. JNTFORC Set dt for joint force file. SBTOUT Set dt for seat belt output file. AVSFLT Set dt for AVS database. MOVIE Set dt for MOVIE. MPGS Set dt for MPGS. TPRINT Set dt for thermal file. RESTART INPUT DATA 2 3 4 5 6 7 8 *DATABASE Card Variable 1 DT Type F VARIABLE DESCRIPTION DT Time interval between outputs: EQ.0.0: output interval is unchanged. Remarks: To terminate output to a particular file set DT to a high value. If IACCOP = 2 was specified in *CONTROL_OUTPUT, the best results are obtained in the NODOUT file by keeping the same DT on restart. When DT is changed for NOD- OUT, oscillations may occur around the restart time. If DT is larger than initially specified in the original input file, more memory is required to store the time states for the averaging than was originally allocated. A warning message is printed, and the filtering is applied using the available memory. When DT is smaller than initially specified, more oscillations may appear in the output than earlier in the calculation because the frequency content of the averaged output increases as DT decreases. *DATABASE_BINARY Options for binary output files with the default names given include: D3PLOT Dt for complete output states. D3THDT Dt for time history data for element subsets. D3DUMP Binary output restart files. Define output frequency in cycles RUNRSF Binary output restart file. Define output frequency in cycles. INTFOR Dt for contact surface Interface database. Card 1 2 3 4 5 6 7 8 Variable DT/CYCL Type F VARIABLE DESCRIPTION DT Time interval between outputs. EQ.0.0: Time interval remains unchanged. CYCL Output interval in time steps. EQ.0.0: output interval remains unchanged. *DELETE_OPTION Available options are: ALECPL CONTACT CONTACT_2DAUTO ENTITY PART ELEMENT_BEAM ELEMENT_SHELL ELEMENT_SOLID ELEMENT_TSHELL FSI Purpose: Delete contact surfaces, ALE FSI couplings, parts, or elements by a list of IDs. There are two contact algorithms for two-dimensional problems: the line-to-line contact and the automatic contact defined by part ID's. Each uses their own numbering. This ID Cards. the ALECPL, CONTACT, format applies CONTACT_2DAUTO, ENTITY, FSI and PART options. Include as many cards as necessary to input desired IDs. This input ends at the next keyword (“*”) card. card 1 to Card 1 Variable ID1 2 ID2 3 ID3 4 ID4 5 ID5 6 ID6 7 ID7 8 ID8 Type I I I I I I I I VARIABLE DESCRIPTION IDn Contact ID/Coupling ID/Part ID Remarks: The FSI option corresponds to ALE couplings defined with *CONSTRAINED_LA- GRANGE_IN_SOLID. The ALECPL option corresponds to ALE couplings defined with *ALE_COUPLING_NODAL_CONSTRAINT. For CONTACT, FSI, and ALECPL options, a negative ID implies that the absolute value gives the contact sur- face/FSI/ALECPL coupling which is to be activated. Element set cards. This card 1 format applies to the four ELEMENT options. This input ends at the next keyword (“*”) card. Card 1 2 3 4 5 6 7 8 Variable ESID Type I VARIABLE ESID DESCRIPTION Element set ID, see *SET_SOLID, *SET_BEAM, *SET_SHELL, *SET_TSHELL. *INTERFACE_SPRINGBACK_LSDYNA Purpose: Define a material subset for output to a stress initialization file “dynain”. The dynain file contains keyword commands that can be included in a subsequent input deck to initialize deformation, stress, and strain in parts. This file can be used, for example, to do an implicit springback analysis after an explicit forming analysis. Part Set ID Cards. Card 1 1 2 3 4 5 6 7 8 Variable PSID NSHV Type I I Constraint Cards. Optional cards that list of nodal points that are constrained in the dynain file. This input ends at the next keyword (“*”) card. 4 5 6 7 8 Card 2 1 Variable NID Type I 2 TC F Default none 0. 3 RC F 0. VARIABLE DESCRIPTION PSID NSHV Part set ID for springback, see *SET_PART. If NSHV Number of shell or solid history variables (beyond the six stresses and effective plastic strain) to be initialized in the interface file. For solids, one additional state variable (initial volume) is also written. is nonzero, the element formulations, calculational units, and constitutive models should not change between runs. If NHSV exceeds the number of integration point history variables required by the constitutive model, only the number required is written; therefore, if in doubt, set NHSV to alarge number. NID Node ID VARIABLE DESCRIPTION TC Translational constraint: EQ.0: no constraints, EQ.1: constrained x displacement, EQ.2: constrained y displacement, EQ.3: constrained z displacement, EQ.4: constrained x and y displacements, EQ.5: constrained y and z displacements, EQ.6: constrained z and x displacements, EQ.7: constrained x, y, and z displacements. RC Rotational constraint: EQ.0: no constraints, EQ.1: constrained x rotation, EQ.2: constrained y rotation, EQ.3: constrained z rotation, EQ.4: constrained x and y rotations, EQ.5: constrained y and z rotations, EQ.6: constrained z and x rotations, EQ.7: constrained x, y, and z rotations. *RIGID_DEFORMABLE_OPTION Available options include: CONTROL D2R (Deformable to rigid part switch) R2D (Rigid to deformable part switch) Purpose: Define parts to be switched from rigid to deformable and deformable to rigid in a restart. It is only possible to switch parts on a restart if part switching was activated in the time zero analysis. See *DEFORMABLE_TO_RIGID for details of part switching. *RIGID_DEFORMABLE_CONTROL Card 1 2 3 4 5 6 7 8 Variable NRBF NCSF RWF DTMAX Type Default I 0 I 0 I 0 F none VARIABLE NRBF DESCRIPTION Flag to delete or activate nodal rigid bodies. If nodal rigid bodies or generalized, weld definitions are active in the deformable bodies that are switched to rigid, then the definitions should be deleted to avoid instabilities: EQ.0: no change, EQ.1: delete, EQ.2: activate. NCSF Flag to delete or activate nodal constraint set. If nodal constraint/spot weld definitions are active in the deformable bodies that are switched to rigid, then the definitions should be deleted to avoid instabilities: EQ.0: no change, EQ.1: delete, EQ.2: activate. RWF Flag to delete or activate rigid walls: EQ.0: no change, EQ.1: delete, EQ.2: activate. DTMAX Maximum permitted time step size after restart. *RIGID_DEFORMABLE_D2R Part ID Cards. Include one card for each part. This input ends at the next keyword (“*”) card. Card 1 1 2 3 4 5 6 7 8 Variable PID MRB Type I Default none I 0 VARIABLE DESCRIPTION PID MRB Part ID of the part which is switched to a rigid material. Part ID of the master rigid body to which the part is merged. If zero, the part becomes either an independent or master rigid body. *RIGID_DEFORMABLE_R2D Termination of this input is when the next “*” card is read. Part ID Cards. Include one card for each part. This input ends at the next keyword (“*”) card. Card 1 1 2 3 4 5 6 7 8 Variable PID Type I Default none VARIABLE DESCRIPTION PID Part ID of the part which is switched to a deformable material. *STRESS_INITIALIZATION_{OPTION} This keyword causes a full deck restart. For a full deck restart the input deck must contain the full model. The stress initialization feature allows all or selected parts to be initialized from the previous calculation using data from the d3dump or runrsf databases. The options that are available with this keyword are: <BLANK> DISCRETE SEATBELT Optional Part Cards. If no part cards are included in the deck then all parts, seatbelts and discrete parts in the new input deck that existed in the previous input deck (with or without the same part IDs) are initialized from the d3dump or runrsf database. Otherwise for each part to be initialized from the restart data include an addition card in format 1. This input terminates at the next keyword (“*”) card. Card 1 1 2 3 4 5 6 7 8 Variable PIDO PIDN Type I I Default none PIDO VARIABLE DESCRIPTION PIDO PIDN Old part ID, see *PART. New part ID, see *PART: EQ.0: New part ID is the same as the old part ID. Remarks: If one or more of the above cards are defined then discrete and seatbelt elements will not be initialized unless the additional option cards *STRESS_INITIALIZATION_DIS- CRETE and *STRESS_INITIALIZATION_SEATBELT are defined. *STRESS_INITIALIZATION_DISCRETE Initialize all discrete parts from the old parts. No further input is required with this card. This card is not required if *STRESS_INITIALIZATION is specified without further input. *STRESS_INITIALIZATION_SEATBELT Initialize all seatbelt parts from the old parts. No further input is required with this card. This card is not required if *STRESS_INITIALIZATION is specified without further input. RESTART INPUT DATA Purpose: Stops the job depending on some displacement conditions. Available options include: NODE BODY Caution: The inputs are different for the nodal and rigid body stop conditions. The nodal stop condition works on the global coordinate position, while the body stop condition works on the relative global translation. The number of termination conditions cannot exceed the maximum of 10 or the number specified in the original analysis. The analysis terminates for *TERMINATION_NODE when the current position of the node specified reaches either the maximum or minimum value (stops 1, 2 or 3), or picks up force from any contact surface (stop 4). For *TERMINATION_BODY the analysis terminates when the center of mass displacement of the rigid body specified reaches either the maximum or minimum value (stops 1, 2 or 3) or the displacement magnitude of the center of mass is exceeded (stop 4). If more than one condition is input, the analysis stops when any of the conditions is satisfied. NOTE: This input completely overrides the existing termi- nation conditions defined in the time zero run. Termination by other means is controlled by the *CONTROL_TERMINATION control card. Node/Part Cards. Include an additional card in format 1 for each node or part with a termination criterion Card 1 2 3 4 5 6 7 8 Variable NID/PID STOP MAXC MINC Type I I Default none none F - F - For the NODE option: VARIABLE DESCRIPTION NID STOP Node ID Stop criterion: EQ.1: global x direction, EQ.2: global y direction, EQ.3: global z direction, EQ.4: stop if node touches contact surface. MAXC MINC Maximum (most positive) coordinate, options 1, 2 and 3 above only. Minimum (most negative) coordinate, options 1, 2 and 3 above only. For the BODY option: VARIABLE DESCRIPTION PID Part ID of rigid body VARIABLE DESCRIPTION STOP Stop criterion: EQ.1: global x direction, EQ.2: global y direction, EQ.3: global z direction, EQ.4: stop if displacement magnitude is exceeded. MAXC Maximum (most positive) displacement, options 1, 2, 3 and 4: EQ.0.0: MAXC set to 1.0e21 MINC Minimum (most negative) displacement, options 1, 2 and 3 above only: EQ.0.0: MINC set to -1.0e21 *TITLE Purpose: Define job title. Card 1 2 3 4 5 6 7 8 Variable Type Default TITLE C LS-DYNA USER INPUT VARIABLE DESCRIPTION TITLE Heading to appear on output. REFERENCES REFERENCES Abbo, A.J., and S.W. Sloan, “A Smooth Hyperbolic Approximation to the Mohr- Coulomb Yield Criterioin,” Computers and Structures, Vol. 54, No. 1, (1995). Allen, D.J., Rule, W.K., Jones, S.E., “Optimizing Material Strength Constants Numerically Extracted from Taylor Impact Data”, Experimental Mechanics, Vol. 37, No 3, September (1997). Allman, D.J., “A Compatible Triangular Element Including Vertex Rotations for Plane Elasticity Analysis,” Computers and Structures, 19, 1-8, (1984). Anagonye, A.U. and J.T. Wang, “A Semi-Empirical Method for Estimating the Effective Leak and Vent Areas of an Airbag”, AMD-Vol. 237/BED-Vol. 45, pp. 195-217, (1999). Anand, L. and M.E. Gurtin, “A theory of amorphous solids undergoing large deformations, with application to polymeric glasses,” International Journal of Solids and Structures, 40, pp. 1465-1487 (2003) Aretz, H. “Applications of a New Plane Stress Yield Function to Orthotropic Steel and Aluminum Sheet Metals,” Modeling and Simulation in Materials Science and Engineering, 12, 491-509 (2004). Argon, AS., “A theory for the low-temperature plastic deformation of glassy polymers”, Philosophical Magazine, 28, 839-865 (1973). Armstrong, P.J., and Frederick, C.O., “A Mathematical Representation of the Multiaxial Bauschinger Effect,” CEGB Report, RD/B/N731, Berkeley Nuclear Laboratories (1966). Arruda, E. and M. Boyce, “A Three-Dimensional Constitutive Model for the Large Stretch Behavior of Rubber Elastic Materials,” Journal of the Mechanics and Physics of Solids, Vol. 41, No. 2, pp. 389-412, (1993). Auricchio, F., R.L. Taylor and J. Lubliner, “Shape-memory alloys: macromodeling and numerical simulations of the superelastic behavior”, Computer Methods in Applied Mechanics and Engineering, vol. 146, pp. 281-312, (1997). Auricchio, F. and R.L. Taylor, “Shape-memory alloys: modeling and numerical simulations of the finite-strain superelastic behavior”, Computer Methods in Applied Mechanics and Engineering, vol. 143, pp. 175-194, (1997). Bahler AS: The series elastic element of mammalian skeletal muscle. Am J Physiol 213:1560-1564, (1967). REFERENCES Baker, E.L., “An Explosives Products Thermodynamic Equation of State Appropriate for Material Acceleration and Overdriven Detonation: Theoretical Background and Fourmulation,” Technical Report ARAED-TR-911013, U.S. Army Armament Research, Development and Engineering Center, Picatinney Arsenal, New Jersey, 1991). Baker, E.L. and J. Orosz, J., “Advanced Warheads Concepts: An Advanced Equation of State for Overdriven Detonation,” Technical Report ARAED-TR-911007, U.S. Army Armament Research, Development and Engineering Center, Picatinney Arsenal, New Jersey, (1991). Baker, E.L. and L.I. Stiel, “Improved Quantitative Explosive Performance Prediction Using Jaguar,” 1997 Insensitive Munitions and Energetic Materials Technology Symposium, Tampa, FL, (1997). Bammann, D.J. and E.C. Aifantis, “A Model for Finite-Deformation Plasticity,” Acta Mechanica, 70, 1-13 (1987). Bammann, D.J. and G. Johnson, “On the Kinematics of Finite-Deformation Plasticity,” Acta Mechanica, 69, 97-117 (1987). Bammann, D.J., “Modeling the Temperature and Strain Rate Dependent Large Deformation of Metals,” Proceedings of the 11th US National Congress of Applied Mechanics, Tuscon, AZ, (1989). Bammann, D.J., M.L. Chiesa, A. McDonald, W.A. Kawahara, J.J. Dike, and V.D. Revelli, “Predictions of Ductile Failure in Metal Structures,” in AMD-Vol. 107, Failure Criteria and Analysis in Dynamic Response, Edited by. H.E. Lindberg, 7-12, (1990). Bandak, F.A., private communications, U.S. Dept. of Trans., Division of Biomechanics Research, 400 7th St., S.W. Washington, D.C. 20590 (1991). Bansal, S., Mobasher, B., Rajan, S., and Vintilescu, I., “Development of Fabric Constitutive Behavior for Use in Modeling Engine Fan Blade-Out Events.” J. Aerosp. Eng. 22, SPECIAL ISSUE: Ballistic Impact and Crashworthiness Response of Aerospace Structures, 249–259, (2009). Barlat, F. and J. Lian, “Plastic Behavior and Stretchability of Sheet Metals. Part I: A Yield Function for Orthotropic Sheets Under Plane Stress Conditions,” Int. J. of Plasticity, Vol. 5, pp. 51-66 (1989). Barlat, F., D.J. Lege, and J.C. Brem, “A Six-Component Yield Function for Anisotropic Materials,” Int. J. of Plasticity, 7, 693-712, (1991). Barlat, F., Y. Maeda, K. Chung, M. Yanagawa, J.C. Brem, Y. Hayashida, D.J. Lege, K. Matsui, S.J. Murtha, S. Hattori, R.C. Becker, and S. Makosey, “Yield Function REFERENCES Development for Aluminum Alloy Sheets”, J. Mech. Phys. Solids, Vol. 45, No. 11-12, 1727-1763, (1997). Barlat, F., Brem, J.C., Yoon, J.W., Chung, K., Dick, R.E., Lege, D.J., Pourboghrat, F., Choi, S.H., Chu, E., “Plane Stress Yield Function for Aluminum Alloy Sheets – Part 1: Theory, Int. J. Plast. 19, 1-23, (2003). Basu, U., “Explicit finite element perfectly matched layer for transient three- dimensional elastic waves,” International Journal for Numerical Methods in Engineering, vol. 77, pp. 151–176, (2009). Basu, U. and Chopra, A.K., “Perfectly matched time-harmonic elastodynamics finite-element implementation,” Computer Methods in Applied Mechanics and Engineering, vol. 192, pp. 1337–1375, (2003). of unbounded domains for and theory layers Basu, U. and Chopra, A.K., “Perfectly matched layers for transient elastodynamics of unbounded domains,” International Journal for Numerical Methods in Engineering, vol. 59, pp. 1039–1074, (2004). Erratum: Ibid. vol. 61, pp. 156–157, (2004). Bathe, K.-J. Conserving energy and momentum in nonlinear dynamics: A simple implicit time integration scheme, Computers and Structures, 85, 437-445 (2007). Bathe, K.-J. and Dvorkin, E.N. A four node plate bending element based on Mindlin- Reissner plate theory and a mixed interpolation, Int. J. Num. Meth. Eng., 21, 367-383 (1985). Bathe, K-J. and Nooh, G. Insight into an implicit time integration scheme for structural dynamics, Computers and Structures, 98/99, 1-6 (2012). Batoz, J.L. and Ben Tahar, M. Evaluation of a new quadrilateral thin plate bending element, Int. J. Num. Meth. Eng., 18, 1644-1677 (1982). Batoz, J.-L. and M. Ben Tahar, Evaluation of a new quadrilateral thin plate bending element, International Journal for Numerical Methods in Engineering, 18, (1982), 1655-1677. Bazeley, G.P., W.K. Cheung, R.M. Irons, and O.C. Zienkiewicz, “Triangular Elements in Plate Bending-Confirming and Nonconforming Solutions in Matrix Methods and Structural Mechanics,” Proc. Conf. on Matrix Methods in Structural Analysis, Rept. AFFDL-R-66-80, Wright Patterson AFB, 547-576 (1965). Belytschko, T. and Bindeman, L. P. “Assumed Strain Stabilization of the Eight Node Hexahedral Element,” Comp. Meth. Appl. Mech. Eng. 105, 225-260 (1993). REFERENCES Belytschko, T.B. and A.H. Marchertas, “Nonlinear Finite Element Method for Plates and its Application to the Dynamic Response of Reactor Fuel Subassemblies,” Trans, ASME J. Pressure Vessel Tech., 251-257 (1974). Belytschko, T.B. and C.S. Tsay, “Explicit Algorithms for Nonlinear Dynamics of Shells,” AMD-Vol.48, ASME, 209-231 (1981). Belytschko, T.B. and C.S. Tsay, “Explicit Algorithms for Nonlinear Dynamics of Shells,” Comp. Meth. Appl. Mech. Eng., 43, 251-276, (1984). Belytschko, T.B. and C.S. Tsay, “A Stabilization Procedure for the Quadrilateral Plate Element with One-Point Quadrature,” Int. J. Num. Method. Eng., 19, 405-419 (1983). Belytschko, T.B., H. Stolarski, and N. Carpenter, “A C° Triangular Plate Element with One-Point Quadrature,” Int. J. Num. Meth. Eng., 20, 787-802 (1984). Belytschko, T.B., I. Yeh, “The Splitting Pinball Method for Contact-Impact Problems,” Comp. Meth. Appl. Mech. Eng., 105, 375-393, (1993). Belytschko, T.B., L. Schwer, and M.J. Klein, “Large Displacement Transient Analysis of Space Frames,” Int. J. Num. Eng., 11, 65-84 (1977). Benson, D.J. and J.O. Hallquist, “A Simple Rigid Body Algorithm for Structural Dynamics Programs,” Int. J. Numer. Meth. Eng., 22, (1986). Benson, D.J. and J.O. Hallquist, “A Single Surface Contact Algorithm for the Postbuckling Analysis of Shell Structures,” Comp. Meths. Appl. Mech. Eng., 78, 141-163 (1990). Benzeggagh, M.L. and Kenane, M., “Measurement of Mixed-mode Delamination Fracture Toughness of Unidirectional Glass/Epoxy Composites with Mixed- mode Bending Apparatus,” Composites Science and Technology, 56, 439-449 (1996). Berstad, T., “Material Modeling of Aluminium for Crashworthiness Analysis”, Dr.Ing. Dissertation, Department of Structural Engineering, Norwegian University of Science and Technology, Trondheim, Norway, (1996). Berstad, T., Hopperstad, O.S., Lademo, O.-G. and Malo, K.A., “Computational Model of Ductile Damage and Fracture in Shell Analysis”, Second European LS-DYNA Conference, Gothenburg, Sweden, (1999). Berstad, T., Lademo, O.-G., Pedersen, K.O. and Hopperstad, O.S., “Formability modeling with LS-DYNA”, 8th International LS-DYNA User’s Conference, Detroit, May 3-5, 2004. REFERENCES Berstad, T., Langseth, M. and Hopperstad, O.S., “Elasto-viscoplastic Constitutive Models in the Explicit Finite Element Code LS-DYNA3D,” Second International LS-DYNA3D conference, San Francisco, (1994). Bergström, J.S. and M.C. Boyce, “Constitutive modeling of the large strain time- dependent behavior of elastomers” J. Mech. Phys. Solids, 46, 931-954 (1998). Bielak, J. and Christiano, P., “On the effective seismic input for non-linear soil-structure interaction systems,” Earthquake Engineering and Structural Dynamics, vol. 12, pp. 107–119, (1984). Bier, M., Sommer, S., “Simplified modeling of self-piercing riveted joints for crash simulation of *CONSTRAINED_INTERPOLATION_SPOTWELD”. 9th European LS-DYNA Conference, Manchester, (2013). modified version with a Bilkhu, S.S., M. Founas, and G.S. Nasholtz, “Material Modeling of Structural Foams in Finite Element Analysis Using Compressive Uniaxial and Triaxial Data,” SAE (Nat. Conf.) Detroit 1993, pp. 4-34. Blatz, P.J., and Ko, W.L., “Application of Finite Element Theory to the Deformation of Rubbery Materials,” Trans. Soc. of Rheology, 6, 223-251 (1962). Borrvall T., Bhalsod D., Hallquist J.O., and Wainscott B., “Current Status of Subcycling and Multiscale Simulations in LS-DYNA”. 13th International LS-DYNA User’s Conference, Dearborn MI, (2014). Boyce, M.C., Parks, D.M., and Argon, A.S., “Large inelastic deformation of glassy polymers. Part I: Rate dependent constitutive model”. Mechanics of Materials, 7, 15-33 (1988). Boyce, M.C., Socrate, C. and Llana, P.G., “Constitutive model for the finite deformation stress-strain behavior of poly(ethylene terephthalate) above the glass transition”. Polymer, 41, 2183-2201 (2000). Brandt, J., On Constitutive Modelling of the Compaction and Sintering of Cemented Carbides, Linköping Studies in Science and Technology, Dissertations 515, 1998. Brekelmans, W.A.M., Scheurs,P.J.G., and de Vree, J.H.P., 1991, “Continuum damage mechanics for softening of brittle materials”, Acta Mechanica, vol 93, pp 133-143 Broadhouse, B.J., “The Winfrith Concrete Model in LS-DYNA3D,” Report: SPD/D(95)363, Structural Performance Department, AEA Technology, Winfrith Technology Centre, U.K. (1995). REFERENCES Broadhouse, B.J. and Neilson, A.J., “Modelling Reinforced Concrete Structures in DYNA3D”, Safety and Engineering Division, United Kingdom Atomic Energy Authority, Winfrith, AEEW-M 2465, 1987. Brode, H.L., “Height of Burst Effects at High Overpressure,” RAND, RM-6301-DASA, DASA 2506, (1970). Brown, B.E. and J.O. Hallquist, “TAURUS: An Interactive Post-Processor for the Analysis Codes NIKE3D, DYNA3D, TACO3D, and GEMINI,” University of California, Lawrence Livermore National Laboratory, Rept. UCID-19392 (1982) Rev. 1 (1984). Bruneau, M., Uang, C.M., Whittaker, A., Ductile Design of Steel Structures, McGraw Hill, (1998). Burton, D.E. et al. “Physics and Numerics of the TENSOR Code,” Lawrence Livermore National Laboratory, Internal Document UCID-19428, (July 1982). Carney, K.S., S.A. Howard, B.A. Miller, and D.J. Benson. “New Representation of in LS-DYNA,” 13th International LS-DYNA Users Conference, Bearings Dearborn, MI, June 8-10, 2014. CEB Code 1993, Comite euro-international du beton, CEB-FIP Model Code 1990, Thomas Telford, London, (1993). Chang, F.K. and K.Y. Chang, “A Progressive Damage Model for Laminated Composites Containing Stress Concentration,” J. of Composite Materials, 21, 834- 855 (1987a). Chang, F.K. and K.Y. Chang, “Post-Failure Analysis of Bolted Composite Joints in Tension or Shear-Out Mode Failure,” J. of Composite Materials, 21 809-823 (1987b). Chang, F.S., “Constitutive Equation Development of Foam Materials,” Ph.D. Dissertation, submitted to the Graduate School, Wayne State University, Detroit, Michigan (1995). Chao, Y. J., Wang, K, Miller, K. W. and Zhu, X. K. “Dynamic Separation of Resistance Spot Welded joints: Part I – Experiments”, Exp Mech, Vol. 50, Issue 7, pp 889-900 (2010). Chen, W.F., and Baladi, G.Y., Soil Plasticity: Theory and Implementation, Elesvier, New York, (1985). Cheng, H., Obergefell, L.A., and Rizer, A., March 1994, “Generator of Body (GEBOD) Manual,” Report No. AL/CF-TR-1994-0051. REFERENCES Chowdhury, S.R. and Narasimhan R., “A Cohesive Finite Element Formulation for Modeling Fracture and Delamination in Solids,” Sadhana, 25(6), 561-587, (2000). Christensen, R.M. “A Nonlinear Theory of Viscoelasticity for Application to Elastomers,” Journal of Applied Mechanics, Volume 47, American Society of Mechanical Engineers, pages 762-768, December 1980. Chu, C.C. and A. Needleman, “Void Nucleation Effects in Biaxially Stretched Sheets”, ASME Journal of Engineering Materials and Technology, 102, 249-256 (1980). Chung, K. and K. Shah, “Finite Element Simulation of Sheet Metal Forming for Planar Anisotropic Metals,” Int. J. of Plasticity, 8, 453-476, (1992). Cochran, S.G. and J. Chan, “Shock Initiation and Detonation Models in One and Two Dimensions,” University of California, Lawrence Livermore National Laboratory, Rept. UCID-18024 (1979). Cook, R. D., Concepts and Applications of Finite Element Analysis, John Wiley and Sons, Inc. (1974). Couch, R., E. Albright, and N. Alexander, The Joy Computer Code, Lawrence Livermore National Laboratory, Internal Document Rept. UCID-19688, (January, 1983). Cowper, G.R. and P.S. Symonds, Strain Hardening and Strain Rate Effects in the Impact Loading of Cantilever Beams, Brown University, Applied Mathematics Report, 1958. CRAY-1 Computer System CFT Reference Manual, Cray Research Incorporated, Bloomington, NM., Publication No. 2240009 (1978). Dal, H. and M. Kaliske, “Bergström-Boyce model for nonlinear finite rubber viscoelasticity: theoretical aspects and algorithmic treatment for the FE method” Computational Mechanics, 44(6), 809-823, (2009). DeRuntz, J.A. Jr., “Reference Material for USA, The Underwater Shock Analysis Code, USA-STAGS, and USA-STAGS-CFA,” Report LMSC-P032568, Computational Mechanics Laboratory, Lockheed Palo Alto Research Laboratory, Palo Alto, CA. (1993). Desai, C.S., and H.J. Siriwardane, Constitutive Laws for Engineering Materials with Emphasis On Geologic Materials, Prentice-Hall, Chapter 10, (1984). Deshpande, V.S. and N.A. Fleck, “Isotropic Models for Metallic Foams,” Journal of the Mechanics and Physics of Solids, 48, 1253-1283, (2000). REFERENCES Dick, R.E., and W.H. Harris, “Full Automated Rezoning of Evolving Geometry Problems,” Numerical Methods in Industrial Forming Processes, Chenot, Wood, and Zienkiewicz, Editors, Bulkema, Rotterdam, 243-248, (1992). Dilger, W.H., R. Koch, and R. Kowalczyk, “Ductility of Plain and Confined Concrete Under Different Strain Rates,” ACI Journal, January-February, (1984). Dobratz, B.M., “LLNL Explosives Handbook, Properties of Chemical Explosives and Explosive Simulants,” University of California, Lawrence Livermore National Laboratory, Rept. UCRL-52997 (1981). Du Bois, P.A., “Numerical Simulation of Strandfoam” Daimler-Chrysler AG Abt. EP/CSV, Report (2001). Dufailly, J., and Lemaitre, J., “Modeling very low cycle fatigue”, International Journal of damage mechanics, 4, pp. 153-170 (1995). Erhart, T., Andrade, F., Du Bois, P., “Short Introductionof a New Generalized Damage Model”, 11th European LS-DYNA Conference, Salzburg, Austria, May 2017. Erhart, T., “A New Feature to Model Shell-Like Structures with Stacked Elements”, 10th European LS-DYNA Conference, Würzburg, Germany, June 2015. Erhart, T., “An Overview of User Defined Interfaces in LS-DYNA”, LS-DYNA Forum, Bamberg, Germany, 2010. Englemann, B. E., R.G. Whirley, and G.L. Goudreau, “A Simple Shell Element Formulation for Large-Scale Elastoplastic Analysis,” CED-Vol. 3. Analytical and Computational Models of Shells, A.K. Noor, T. Belytschko, and J.C. Simo, Editors, 1989, pp. 399-416. Faßnacht, W., “Simulation der Rißbildung in Aluminiumgußbauteilen,” Dissertation, Technishe Universität Darmstadt, (1999). Feng, W.W. and Hallquist, J.O., “On Constitutive Equations for Elastomers and Elastomeric Foams”, The 4th European LS-DYNA Conference, D-II-15, Ulm, Germany, May 2003. Feucht, M., “Ein gradientenabhängiges Gursonmodell zur Beshreibung duktiler Schädigung mit Entfestigung,” Dissertation, Technishe Universität Darmstadt, (1998). Fiolka, M. and Matzenmiller, A., “Delaminationsberechnung von Faserverbund- strukturen”, PAMM Proc. Appl. Math. Mech. 5, S.393-394 (2005). REFERENCES Flanagan, D.P. and T. Belytschko, “A Uniform Strain Hexahedron and Quadrilateral and Orthogonal Hourglass Control,” Int. J. Numer. Meths. Eng., 17, 679-706 (1981). Fleischer, M., Borrvall, T. and Bletzinger, K-U., “Experience from using recently implemented enhancements for Material 36 in LS-DYNA 971 performing a virtual tensile test”, 6th European LS-DYNA Users Conference, Gothenburg, 2007. Forghani A., “A Non-Local Approach to Simulation of Damage in Composite Structures”, PhD Thesis, Department of Civil Engineering, The University of British Columbia,, Vancouver, Canada, (2011). Forghani A., Zobeiry N., Vaziri R., Poursartip A., and Ellyin F., “A Non-Local Approach to Simulation of Damage in Laminated Composites.” Proc., ASC/CANCOM Conference, Montreal, Canada (2011b). Forghani A., Zobeiry N., Poursartip A., and Vaziri R., “A Structural Modeling Framework for Prediction of Damage Development and Failure of Composite Laminates”. Accepted for publication in Composites Sci. Technol. Freed AD., Einstein DR. and Vesely I., “Invariant Formulation for Dispersed Transverse Isotropy in Aortic Heart Valves – An Efficient Means for Modeling Fiber Splay”, Biomechan Model Mechanobiol, 4, 100-117 (2005) Fung, Y.C., Biomechanics, Springer, New York, 1993. Fung, Y.C., Foundations of Solid Mechanics, Prentice Hall, Inc., Englewood Cliffs, New Jersey, 1965. Gerlach, S., Fiolka M. and Matzenmiller, A., Modelling and analysis of adhesively bonded joints with interface elements for crash analysis, 4. LS-DYNA Forum, 20- 21, (2005) Bamberg, DYNAmore GmbH, Stuttgart. Ginsberg, M. and J. Johnson, “Benchmarking the Performance of Physical Impact Simulation Software on Vector and Parallel Computers,” Applications Track of Supercomputing, IEEE monograph, Computer Society Press, March, 1989. Giroux, E.D. HEMP User’s Manual, University of California, Lawrence Livermore National Laboratory, Rept. UCRL-51079 (1973). Goldberg, R., and D. Stouffer, “High Strain Rate Dependent Modeling Polymer Matrix Composites,” NASA/TM-1999-209433 (1999). Goudreau, G.L. and J.O. Hallquist, “Recent Developments in Large Scale Finite Element Lagrangian Hydrocode Technology,” J. Comp. Meths. Appl. Mechs. Eng., 30 (1982). REFERENCES Goldak, J., Chakravarti, A., and Bibby, M., “A New Finite Element Model for Welding Heat Sources,” Metallurgical Transactions B, vol. 15B, pp. 299-305, June, 1984. Govindjee, S., Kay, J.G., and Simo, J.C. [1994], Anisotropic Modeling and Numerical Simulation of Brittle Damage in Concrete, Report No. UCB/SEMM-94/18, Department of Civil Engineering, University of California, Berkeley, CA 94720. Govindjee, S., Kay, J.G., and Simo, J.C. [1995], “Anisotropic Modeling and Numerical Simulation of Brittle Damage in Concrete,” Int. J. Numer. Meth. Engng, 38, 3611-3633. Graefe, H., W. Krummheuer, and V. Siejak, “Computer Simulation of Static Deployment Tests for Airbags, Air Permeability of Uncoated Fabrics and Steady State Measurements of the Rate of Volume Flow Through Airbags,” SAE Technical Paper Series, 901750, Passenger Car Meeting and Expositition, Dearborn, Michigan, September 17-20, 1990. Gran, J.K. and P.E. Senseny, “Compression Bending of Scale-Model Reinforced- Concrete Walls,” ASCE Journal of Engineering Mechanics, Volume 122, Number 7, pages 660-668, July (1996). Grassl, P., U. Nyström, R. Rempling, and K. Gylltoft, “A Damage-Plasticity Model for the Dynamic Failure of Concrete”, 8th International Conference on Structural Dynamics, Leuven, Belgium, March (2011). Grassl, P., D. Xenos, U. Nyström, R. Rempling, and K. Gylltoft, “CDPM2: A damage- plasticity approach to modelling the failure of concrete”, International Journal of Solids and Structures, Vol. 50, Issue 24, pp. 3805-3816, (2013). Grassl, P. and M. Jirásek, “Damage-Plastic Model for Concrete Failure”, International Journal of Solids and Structures, Vol. 43, Issues 22-23, pp. 7166-7196, November (2006). Guccione, J., A. McCulloch, and L. Waldman, “Passive Material Properties of Intact Ventricular Myocardium Determined from a Cylindrical Model”, ASME Journal of Biomechanical Engineering, Vol. 113, pages 42-55, (1991). Guccione JM, Waldman LK, McCulloch AD., “Mechanics of Active Contraction in Cardiac Muscle: Part II – Cylindrical Models of the Systolic Left Ventricle”, J. Bio Mech, 115, 82-90, (1993). Gurson, A.L., Plastic Flow and Fracture Behavior of Ductile Materials Incorporating Void Nucleation, Growth, and Interaction, Ph.D. Thesis, Brown University, (1975). REFERENCES Gurson, A.L., “Continuum Theory of Ductile Rupture by Void Nucleation and Growth: Part I - Yield Criteria and Flow Rules for Porous Ductile Media”, J. of Eng. Materials and Technology, (1977). Hallquist, J.O., Preliminary User’s Manuals for DYNA3D and DYNAP (Nonlinear Dynamic Analysis of Solids in Three Dimension), University of California, Lawrence Livermore National Laboratory, Rept. UCID-17268 (1976) and Rev. 1 (1979).[a] Hallquist, J.O., A Procedure for the Solution of Finite Deformation Contact-Impact Problems by the Finite Element Method, University of California, Lawrence Livermore National Laboratory, Rept. UCRL-52066 (1976). Hallquist, J.O., “A Numerical Procedure for Three-Dimensional Impact Problems,” American Society of Civil Engineering, Preprint 2956 (1977). Hallquist, J.O., “A Numerical Treatment of Sliding Interfaces and Impact,” in: K.C. Park and D.K. Gartling (eds.) Computational Techniques for Interface Problems, AMD Vol. 30, ASME, New York (1978). Hallquist, J.O., NIKE2D: An Implicit, Finite-Element Code for Analyzing the Static and Dynamic Response of Two-Dimensional Solids, University of California, Lawrence Livermore National Laboratory, Rept. UCRL-52678 (1979).[b] Hallquist, J.O., User's Manual for DYNA2D – An Explicit Two-Dimensional Hydrodynamic Finite Element Code with Interactive Rezoning, University of California, Lawrence Livermore National Laboratory, Rept. UCID-18756 (1980). Hallquist, J.O., User's Manual for DYNA3D and DYNAP (Nonlinear Dynamic Analysis of Solids in Three Dimensions), University of California, Lawrence Livermore National Laboratory, Rept. UCID-19156 (1981).[a] Hallquist, J. O., NIKE3D: An Implicit, Finite-Deformation, Finite-Element Code for Analyzing the Static and Dynamic Response of Three-Dimensional Solids, University of California, Lawrence Livermore National Laboratory, Rept. UCID- 18822 (1981).[b] Hallquist, J.O., DYNA3D User's Manual (Nonlinear Dynamic Analysis of Solids in Three Dimensions), University of California, Lawrence Livermore National Laboratory, Rept. UCID-19156 (1982; Rev. 1: 1984; Rev. 2: 1986). Hallquist, J.O., Theoretical Manual for DYNA3D, University of California, Lawrence Livermore National Laboratory, Rept. UCID-19501 (March, 1983). Hallquist, J.O., DYNA3D User's Manual (Nonlinear Dynamic Analysis of Solids in Three Dimensions), University of California, Lawrence Livermore National Laboratory, Rept. UCID-19156 (1988, Rev. 4). REFERENCES Hallquist, J.O., LS-DYNA User's Manual (Nonlinear Dynamic Analysis of Solids in Three Dimensions), Livermore Software Technology Corporation, Rept. 1007 (1990). Hallquist, J.O., D.J. Benson, and G.L. Goudreau, “Implementation of a Modified Hughes-Liu Shell into a Fully Vectorized Explicit Finite Element Code,” Proceedings of the International Symposium on Finite Element Methods for Nonlinear Problems, University of Trondheim, Trondheim, Norway (1985). Hallquist, J.O. and D.J. Benson, “A Comparison of an Implicit and Explicit Implementation of the Hughes-Liu Shell,” Finite Element Methods for Plate and Shell Structures, T.J.R. Hughes and E. Hinton, Editors, 394-431, Pineridge Press Int., Swanea, U.K. (1986). Hallquist, J.O. and D.J. Benson, DYNA3D User’s Manual (Nonlinear Dynamic Analysis of Solids in Three Dimensions), University of California, Lawrence Livermore National Laboratory, Rept. UCID-19156 (Rev. 2: 1986; Rev. 3: 1987). Hallquist, J.O., D.W. Stillman, T.J.R. Hughes, C. and Tarver,”Modeling of Airbags Using MVMA/DYNA3D,” LSTC Report (1990). Hashin, Z, “Failure Criteria for Unidirectional Fiber Composites,” Journal of Applied Mechanics, 47, 329 (1980). Haßler, M., Schweizerhof, K., “On the influence of fluid-structure-interaction on the static stability of thin walled shell structures”, International Journal of Structural Stability, Vol. 7, pp. 313–335, (2007). Haßler, M., Schweizerhof, K., “On the static interaction of fluid and gas loaded multi- chamber systems in a large deformation finite element analysis”, Computer Methods in Applied Mechanics and Engineering, Vol. 197, pp. 1725–1749, (2008). Hänsel, C., P. Hora, and J. Reissner, “Model for the Kinetics of Strain-Induced Martensitic Phase Transformation at Isothermal Conditions for the Simulation of Sheet Metal Forming Processes with Metastable Austenitic Steels,” Simulation of Materials Processing: Theory, Methods, and Applications, Huétink and Baaijens (eds), Balkema, Rotterdam, (1998). Haward, R.N., and Thackray, G., “The use of a mathematical model to describe isothermal stress-strain curves in glassy thermoplastics”. Proc Roy Soc A, 302, 453-472 (1968). Herrmann, L.R. and F.E. Peterson, “A Numerical Procedure for Viscoelastic Stress Analysis,” Seventh Meeting of ICRPG Mechanical Behavior Working Group, Orlando, FL, CPIA Publication No. 177, 1968. REFERENCES Hill A.V., “The heat of shortening and the dynamic constants of muscle,” Proc Roy Soc B126:136-195, (1938). Hill, R., “A Theory of the Yielding and Plastic Flow of Anisotropic Metals,” Proceedings of the Royal Society of London, Series A., Vol. 193, pp. 281-197 (1948). Hill, R., “Aspects of Invariance in Solid Mechanics,” Advances in Applied Mechanics, Vol. 18, pp. 1-75 (1979). Hill, R., “Constitutive Modeling of Orthotropic Plasticity in Sheet Metals,” J. Mech. Phys. Solids, Vol. 38, No. 3, 1989, pp. 405-417. Hippchen, P., Merklein, M., Lipp, A., Fleischer, M., Grass, H., Craighero, P., “Modelling kinetics of phase transformation for the indirect hot stamping process”, Key Engineering Materials, Vol. 549, pages 108-116, (2013). Hippchen, P., “Simulative Prognose der Geometrie indirekt pressgehärteter Karosseriebauteile für die industrielle Anwendung”, Dissertation, Technische Fakultät der Friedrich-Alexander Universität Erlangen-Nürnberg, Meisenbach Verlag Bamberg, Band 249, (2014). Hirth, A., P. Du Bois, and K. Weimar, “Improvement of LS-DYNA Material Law 83 (Fu Chang) for the Industrial Simulation of Reversible Energy-Absorbing Foams,” CAD-FEM User's Meeting, Bad Neuenahr - Ahrweiler, Germany, October 7-9, Paper 2-40, (1998). Hollenstein M., M. Jabareen, and M.B. Rubin, “Modelling a smooth elastic-inelastic transition with a strongly objective numerical integrator needing no iteration”, Comput. Mech., Vol. 52, pp. 649-667, DOI 10.1007/s00466-013-0838-7 (2013). Hollenstein M., M. Jabareen, and M.B. Rubin, “Erratum to: Modelling a smooth elastic- inelastic transition with a strongly objective numerical integrator needing no iteration”, Comput. Mech., DOI 10.1007/s00466-014-1099-9 (2014). Holmquist, T.J., G.R. Johnson, and W.H. Cook, “A Computational Constitutive Model for Concrete Subjected to Large Strains, High Strain Rates, and High Pressures”, Proceedings 14th International Symposium on Ballistics, Quebec, Canada, pp. 591-600, (1993). Hopperstad, O.S. and Remseth, S.,” A return Mapping Algorithm for a Class of Cyclic Plasticity Models”, International Journal for Numerical Methods in Engineering, Vol. 38, pp. 549-564, (1995). Huang, Yuli, private communication, Livermore, (2006). Hughes, T.J.R. and E. Carnoy, “Nonlinear Finite Element Shell Formulation Accounting for Large Membrane strains,” AMD-Vol.48, ASME, 193-208 (1981). REFERENCES Hughes, T.J.R. and W.K. Liu, “Nonlinear Finite Element Analysis of Shells: Part I. Three-Dimensional Shells.” Comp. Meths. Appl. Mechs., 27, 331-362 (1981a). Hughes, T.J.R. and W.K. Liu, “Nonlinear Finite Element Analysis of Shells: Part II. Two-Dimensional Shells.” Comp. Meths. Appl. Mechs., 27, 167-181 (1981b). Hughes, T.J.R., W.K. Liu, and I. Levit, “Nonlinear Dynamics Finite Element Analysis of W. Shells.” Nonlinear Finite Element Analysis in Struct. Wunderlich, E. Stein, and K.J. Bathe, Springer-Verlag, Berlin, 151- 168 (1981c). Mech., Eds. Huh, H., Chung, K., Han, S.S., and Chung, W.J., “The NUMISHEET 2011 Benchmark Study of the 8th International Conference and Workshop on Numerical Simulation of 3D Sheet Metal Forming Processes, Part C Benchmark Problems and Results”, p 171-228, Seoul, Korea, August, 2011. Huh, H. and Kang, W.J., “Crash-Worthiness Assessment of Thin-Walled Structures with the High-Strength Steel Sheet”, Int. Journal of Vehicle Design, Vol. 30, Nos. 1/2 (2002). Ibrahimbegovic, A. and Wilson, E.L. “A unified formulation for triangular and quadrilateral flat shell finite elements with six nodal degrees of freedom”, Comm. Applied Num. Meth, 7, 1-9 (1991). Isenberg, J., Vaughan, D.K., Sandler, I.S., Nonlinear Soil-Structure Interaction, Electric Power Research Institute report EPRI NP-945, Weidlinger Associates (1978). Ivanov, I., and A. Tabiei, “Loosely Woven Fabric Model With Viscoelastic Crimped Fibers for Ballistic Impact Simulations”, IJNME, 57, (2004). Jabareen, M., “Strongly objective numerical implementation and generalization of a unified large inelastic deformation model with a smooth elastic-inelastic transition”, submitted to Int. J. Solids and Struct. (2015). Jabareen, M., and Rubin, M.B., A Generalized Cosserat Point Element (CPE) for Isotropic Nonlinear Elastic Materials including Irregular 3-D Brick and Thin Structures, J. Mech. Mat. And Struct., Vol 3-8, 1465-1498 (2008). Jabareen, M., Hanukah, E. and Rubin, M.B., A Ten Node Tetrahedral Cosserat Point Element (CPE) for Nonlinear Isotropic Elastic Materials, J. Comput. Mech. 52, 257-285 (2013). Johnson, G.C. and D.J. Bammann, “A discussion of stress rates in finite deformation problems,” Int. J. Solids Struct, 20, 725-737 (1984). Johnson, G.R. and W.H. Cook, “A Constitutive Model and Data for Metals Subjected to Large Strains, High Strain Rates and High Temperatures.” Presented at the REFERENCES Seventh International Symposium on Ballistics, The Hague, The Netherlands, April 1983. Johnson, G.R. and T.J. Holmquist, “An Improved Computational Model for Brittle Materials” in High-Pressure Science and Technology - 1993 American Institute of Physics Conference Proceedings 309 (c 1994) pp.981-984 ISBN 1-56396-219-5. Jones, R.M., Mechanics of Composite Materials, Hemisphere Publishing Corporation, New York, (1975). Kenchington, G.J., “A Non-Linear Elastic Material Model for DYNA3D,” Proceedings of the DYNA3D Users Group Conference, published by Boeing Computer Services (Europe) Limited (1988). Key, S.W. HONDO – A Finite Element Computer Program for the Large Deformation Dynamic Response of Axisymmetric Solids, Sandia National Laboratories, Albuquerque, N.M., Rept. 74-0039 (1974). Kolling, S., Haufe, A., Feucht, M., DuBois, P. A. “SAMP-1: A Semi-Analytical Model for the Simulation of Polymers”, 4. LS-DYNA Anwenderforum, October 20-21, Bamberg, Germany, (2005). Kolling, S., Hirth, A., Erhart, and Du Bois P.A., Private Communication, Livermore, California (2006). Krieg, R.D.,A Simple Constitutive Description for Cellular Concrete, Sandia National Laboratories, Albuquerque, NM, Rept. SC-DR-72-0883 (1972). Krieg, R.D. and S.W. Key, “Implementation of a Time Dependent Plasticity Theory into Structural Computer Programs,” Vol. 20 of Constitutive Equations in Viscoplasticity: Computational and Engineering Aspects (American Society of Mechanical Engineers, New York, N.Y., pp. 125-137 (1976). Lademo, O.G., Berstad, T., Tryland, T., Furu, T., Hopperstad, O.S. and Langseth, M., “A model for process-based crash simulation”, 8th International LS-DYNA User’s Conference, Detroit, May 3-5, 2004. Lademo, O.G., Hopperstad, O.S., Berstad, T. and Langseth M., “Prediction of Plastic Instability in Extruded Aluminum Alloys Using Shell Analysis and a Coupled Model of Elasto-plasticity and Damage,” Journal of Materials Processing Technology, 2002 (Article in Press). Lademo, O.G., Hopperstad, O.S., Malo, K.A. and Pedersen, K.O., “Modelling of Plastic Anisotropy in Heat-Treated Aluminum Extrusions”, Journal of Materials Processing Technology 125-126, pp. 84-88 (2002). REFERENCES Lee, E.L. and C.M. Tarver, “Phenomenological Model of Shock Initiation in Heterogenous Explosives,” PHYS. Fluids, Vol. 23, p. 2362 (1980). Lee, Y. L. and S Balur of Chrysler Group LLC, “Method of predicting spot weld failure” (Attorney Docket No 708494US2), filed on December 22, 2011 and assigned US Serial No. 13/334,701. Lemaitre, J., A Course on Damage Mechanics, Springer-Verlag, (1992). Lemaitre, J., and Chaboche, J.L., Mechanics of Solid Materials, Cambridge University Press, (1990). Lemmen, P. P. M. and Meijer, G. J., “Failure Prediction Tool Theory and User Manual,” TNO Report 2000-CMC-R0018, (2001). Lewis, B.A., “Developing and Implementing a Road Side Safety Soil Model into LS- DYNA,” FHWA Research and Development Turner-Fairbank Highway Research Center, (1999). Li, Y.H. and Sellars, C.M., “Modeling Deformation Behavior of Oxide Scales and their Effects on Interfacial Heat Transfer and Friction during Hot Steel Rolling”, Proc. Of the 2nd Int. Conf. Modeling of Metals Rolling Processes, The Insitute of Materials, Londong, UK, 192-201 (1996). Lindström P.R.M, “DNV Platform of Computational Welding Mechanics”, Proc. of Int. Inst. Welding 66th Annual Assembly (2013). Lindström, P., "Improved CWM platform for modelling welding procedures and their effects on structural behaviour", PhD Thesis, Production Technology, University West, Trollhättan, Sweden (2015). Lian, W., personal communication: “LS-DYNA Airbag Module Improvement Request”, General Motors Corporation (2000). Y. Luo, “An Efficient 3D Timoshenko Beam Element with Consistent Shape Functions” Adv. Theor. Appl. Mech., 1(3), 95-106, (2008). MADYMO3D USER’S MANUAL, Version 4.3, TNO Road-Vehicles Research Institute, Department of Injury Prevention, The Hague, The Netherlands, (1990). Maimí, P., Camanho, P.P., Mayugo, J.A., Dávila, C.G., “A continuum damage model for composite laminates: Part I – Constitutive model”, Mechanics of Materials, Vol. 39, pp. 897–908, (2007). Maimí, P., Camanho, P.P., Mayugo, J.A., Dávila, C.G., “A continuum damage model for composite laminates: Part II – Computational implementation and validation”, Mechanics of Materials, Vol. 39, pp. 909–919, (2007). REFERENCES Maker, B.N., Private communication Lawrence Livermore National Laboratory, Dr. Maker programmed and implemented the compressible Mooney Rivlin rubber model (1987). Makris N. and Zhang, J., “Time-domain visco-elastic analysis of earth structures,” Earthquake Engineering and Structural Dynamics, vol. 29, pp. 745–768, (2000). Malvar, L.J., Crawford, J.E., Morrill, K.B., K&C Concrete Material Model Release III — Automated Generation of Material Model Input, K&C Technical Report TR-99- 24-B1, 18 August 2000 (Limited Distribution). Malvar, L.J., Crawford, J.E., Wesevich, J.W., Simons, D., “A Plasticity Concrete Material Model for DYNA3D,” International Journal of Impact Engineering, Volume 19, Numbers 9/10, pages 847-873, December 1997. Malvar, L.J., and Ross, C.A., “Review of Static and Dynamic Properties of Concrete in Tension,” ACI Materials Journal, Volume 95, Number 6, pages 735-739, November-December 1998. Malvar, L.J., and Simons,D., “Concrete Material Modeling in Explicit Computations,” Proceedings, Workshop on Recent Advances in Computational Structural Dynamics and High Performance Computing, USAE Waterways Experiment Station, Vicksburg, MS, pages 165-194, April 1996. (LSTC may provide this reference upon request.) Malvar, H.S., Sullivan, G.S., and Wornell, G.W., “Lapped Orthogonal Vector Quantization”, in Proc. Data Compression Conference, Snowbird, Utah, 1996. Marin, E.B., unpublished paper, Sandia National Laboratory, CA (2005). Matzenmiller, A. and Burbulla, F., “ Robustheit und Zuverlässigkeit der Berechnungsmethoden von Klebverbindungen mit hochfesten Stahlblechen unter Crashbedingungen” (2013), http://www.ifm.maschinenbau.uni-kassel.de/ ~amat/publikationen/p75_p828-modellerweiterung.pdf Matzenmiller, A., Lubliner, J., and Taylor, R.L., “A Constitutive Model for Anisotropic Damage in Fiber-Composites,” Mechanics of Materials, Vol. 20, pp. 125-152 (1995). Matzenmiller, A. and J. K. Schweizerhof, “Crashworthiness Considerations of Composite Structures – A First Step with Explicit Time Integration in Nonlinear Computational Mechanics–State-of-the-Art,” Ed. P. Wriggers, W. Wagner, Springer Verlay, (1991). Mauldin, P.J., R.F. Davidson, and R.J. Henninger, “Implementation and Assessment of the Mechanical-Threshold-Stress Model Using the EPIC2 and PINON Computer Codes,” Report LA-11895-MS, Los Alamos National Laboratory (1990). REFERENCES Maurer, A., Gebhardt, M., Schweizerhof, K., “Computation of fluid and/or gas filled inflatable dams“, LS-Dyna Forum, Bamberg, Germany, (2010). McCormick, P.G., “Theory of flow localization due to dynamic strain ageing,” Acta Metallurgica, 36, 3061-3067 (1988). Mi Y., Crisfield, M.A., Davies, A.O. Progressive delamination using interface elements. J Compos Mater, 32(14)1246-72 (1998). Moran, B., Ortiz, M. and Shih, C.F., “Formulation of implicit finite element methods for multiplicative finite deformation plasticity”. Int J for Num Methods in Engineering, 29, 483-514 (1990). de Moura MFSF, Gonçalves, J.P., Marques, A.T., and de Castro, P.T., Elemento finito isoparamétrico de interface para problemas tridimensionais. Revista Internacional de Métodos Numéricos Para Cálculo e Diseño en Ingeniería, 14:447-66 (1996). Murray, Y.D., Users Manual for Transversely Isotropic Wood Model APTEK, Inc., Technical Report to the FHWA (to be published) (2002). Murray, Y.D. and Lewis, B.A., Numerical Simulation of Damage in Concrete APTEK, Inc., Technical Report DNA-TR-94-190, Contract DNA 001-91-C-0075, Defense Nuclear Agency, Alexandria VA 22310. Murray, Y.D., Users Manual for LS-DYNA Concrete Material Model 159, Report No. FHWA-HRT-05-062, Federal Highway Administration, (2007). Murray, Y.D., A. Abu-Odeh, and R. Bligh, Evaluation of Concrete Material Model 159, Report No. FHWA-HRT-05-063, Federal Highway Administration, (2007). Muscolini, G., Palmeri, A. and Ricciardelli, F., “Time-domain response of linear hysteretic systems to deterministic and random excitations,” Earthquake Engineering and Stuctrual Dynamics, vol. 34, pp. 1129–1147, (2005). Nagararaiah, Reinhorn, & Constantinou, “Nonlinear Dynamic Analysis of 3-D Base- Isolated Structures”, Jounal of Structural Engineering Vol 117, No 7, (1991). Nahshon, K. and Hutchinson, J.W., “Modification of the Gurson Model for shear failure”, European Journal of Mechanics A/Solids, Vol. 27, 1-17, (2008). Naik D., Sankaran S., Mobasher D., Rajan S.D., Pereira J.M., “Development of reliable modeling methodologies for fan blade out containment analysis – Part I: Experimental studies”, International Journal of Impact Engineering, Volume 36, Issue 1, Pages 1-11, (2009) Neal, M.O., C-H Lin, and J. T. Wang, “Aliasing Effects on Nodal Acceleration Output International from Nonlinear Finite Element Simulations,” ASME 2000 REFERENCES Mechanical Engineering Congress and Exposition, Orlando, Florida, November 5-10, (2000). Neilsen, M.K., H.S. Morgan, and R.D. Krieg, “A Phenomenological Constitutive Model for Low Density Polyurethane Foams,” Rept. SAND86-2927, Sandia National Laboratories, Albuquerque, N.M., (1987). Nusholtz, G., W. Fong, and J. Wu, “Air Bag Wind Blast Phenomena Evaluation,” Experimental Techniques, Nov.-Dec. (1991). Nusholtz, G., D. Wang, and E.B. Wylie, “Air Bag Momentum Force Including Aspiration,” Preprint, Chrysler Corporation, (1996). Nusholz, private communication, (1996). Nygards, M., M. Just, and J. Tryding, “Experimental and numerical studies of creasing of paperboard,” Int. J. Solids and Struct., 46, 2493-2505 (2009). Ogden, R.W., Non-Linear Elastic Deformations, Ellis Horwood Ltd., Chichester, Great Britian (1984). Oliver, J., “A Consistent Characteristic Length of Smeared Cracking Models,” International Journal for Numerical Methods in Engineering, 28, 461-474 (1989). Papadrakakis, M., “A Method for the Automatic Evaluation of the Dynamic Relaxation Parameters,” Comp. Meth. Appl. Mech. Eng., Vol. 25, pp. 35-48 (1981). Park, R. and Paulay, T., (1975) Reinforced Concrete Structures, J. Wiley and Sons, New York. Park, Y.J., Wen, Y.K, and Ang, A.H-S, “Random Vibration of Hysteretic Systems Under Bi-directional Ground Motions”, Earthquake Engineering and Structural Dynamics, Vol. 14, pp. 543-557 (1986). Penelis, G.G. and Kappos, A.J., Earthquake-Resistant Concrete Structures, E&FN Spon., (1997). Pijaudier-Cabot, G., and Bazant, Z.P., “Nonlocal Damage Theory,” Journal of Engineering Mechanics, ASCE, Vol. 113, No. 10, 1512-1533 (1987). Pinho, S.T., Iannucci, L., Robinson, R., “Physically-based failure models and criteria for laminated fibre-reinforced composites with emphasis on fibre kinking: Part I: Development”, Composties Part A, Vol. 37, 63-73 (2006). Pinho, S.T., Iannucci, L., Robinson, R., “Physically-based failure models and criteria for laminated fibre-reinforced composites with emphasis on fibre kinking: Part II: FE implementation”, Composties Part A, Vol. 37, 766-777 (2006). REFERENCES Porcaro, R., A.G. Hanssen, A. Aalberg and M. Langseth, “The behaviour of aself- piercing riveted connection under quasi-static loading conditions,” Int. J. Solids and Structures, Vol. 43/17, pp. 5110-5131 (2006). Porcaro, R., A.G. Hanssen, A. Aalberg and M. Langseth, “Self-piercing riveting process, an experimental and numerical investigation,” Journal of Materials processing Technology, Vol. 171/1, pp. 10-20 (2006). Porcaro, R., M. Langseth, A.G. Hanssen, H. Zhao, S. Weyer and H. Hooputra, “Crashworthiness of self-piercing riveted connections,” International Journal of Impact Engineering, In press, Accepted manuscript (2007). Puck, A., Kopp, J., Knops, M., “Guidelines for the determination of the parameters in Puck’s action plane strength criterion”, Composites Science and Technology, Vol. 62, 371-378 (2002). Puso, M.A., “A Highly Efficient Enhanced Assumed Strain Physically Stabilized Hexahedral Element”, Int. J. Numer. Meth. Eng., Vol. 49, 1029-1064 (2000). Puso, M.A., and Laursen, T.A., “A Mortar segment-to-segment contact method for large deformation solid mechanics”, Comput. Methods Appl. Mech. Engrg. 193 (2004) 601- 629. Puso, M.A., and Laursen, T.A., “A Mortar segment-to-segment frictional contact method for large deformations”, Comput. Methods Appl. Mech. Engrg. 193 (2004) 4891-4913. Puso, M.A. and Weiss, J.A., “Finite Element Implementation of Anisotropic Quasilinear Viscoelasticity Using a Discrete Spectrum Approximation”, ASME J. Biomech. Engng., 120, 62-70 (1998). Pelessone, D., Private communication, GA Technologies, P.O. Box 85608, San Diego, CA., Telephone No. 619-455-2501 (1986). Quapp, K.M. and Weiss, J.A., “Material Characterization of Human Medial Collateral Ligament”, ASME J. Biomech Engng., 120, 757-763 (1998). Reyes, A., O.S. Hopperstad, T. Berstad, and M. Langseth, Implementation of a Material Model for Aluminium Foam in LS-DYNA, Report R-01-02, Restricted, Department of Structural Engineering, Norwegian University of Science and Technology, (2002). Randers-Pehrson, G. and K. A. Bannister, Airblast Loading Model for DYNA2D and DYNA3D, Army Research Laboratory, Rept. ARL-TR-1310, publicly released with unlimited distribution, (1997). REFERENCES Richards, G.T., Derivation of a Generalized Von Neuman Psuedo-Viscosity with Directional Properties, University of California, Lawrence Livermore National Laboratory, Rept. UCRL-14244 (1965). Riedel W., Thoma K., Hiermaier S. and Schmolinske E., “Penetration of reinforced concrete by BETA-B-500”, in Proc. 9. ISIEMS, Berlin Strausberg, Mai (1999). Riedel W., “Beton unter Dynamischen Lasten – Meso- und Makromechanische Modelle” In: Ernst-Mach-Institut, editor. Freiburg: Fraunhofer IRB, ISBN 3-8167- 6340-5; 2004. Ritto-Corrêa M. and Camotim D., “On the arc-length and other quadratic control methods: Established, less known and new implementation procedures”, Comput. Struct., 86, pp. 1353-1368 (2008). Roussis, P.C., and Constantinou, M.C., “Uplift-restraining Friction Pendulum seismic isolation system”, Earthquake Engineering and Structural Dynamics, 35 (5), 577-593, (2006). Rumpel, T., Schweizerhof, K., “Volume-dependent pressure loading and its influence on the stability of structures“, International Journal for Numerical Methods in Engineering, Vol. 56, pp. 211-238, (2003). Rumpel, T., Schweizerhof, K., “Hydrostatic fluid loading in non-linear finite element analysis“, International Journal for Numerical Methods in Engineering, Vol. 59, pp. 849–870, (2004). Rupp, A., Grubisic, V., and Buxbaum, O., Ermittlung ertragbarer Beanspruchungen am Schweisspunkt auf Basis der ubertragbaren Schnittgrossen, FAT Schriftenreihe 111, Frankfurt (1994). Sala, M.O. Neal, and J.T. Wang, Private Communication, General Motors, May, 2004. Sackett, S.J., “Geological/Concrete Model Development,” Private Communication (1987). Sandler, I.S. and D. Rubin, “An Algorithm and a Modular Subroutine for the Cap Model,” Int. J. Numer. Analy. Meth. Geomech., 3, pp. 173-186 (1979). Schedin, E., Prentzas, L. and Hilding D., “Finite Element Simulation of the TRIP-effect in Austenitic Stainless Steel,” presented at SAE 2004, SAE Technical paper 2004- 01-0885, (2004). Schulte-Frankenfeld N., Deiters, T., “General Introduction to FATXML – data format“, https://www.vda.de/dam/vda/publications/FATXML- Format%20Version%20V1.1/1305643077_de_2066216985.zip, (2016). REFERENCES Schweizerhof, K. and E. Ramm, “Displacement Dependent Pressure Loads in Nonlinear Finite Element Analyses,” Comput. Struct., 18, pp. 1099-1114 (1984). Schwer, L.E., “A Viscoplastic Augmentation of the Smooth Cap Model,” Nuclear Engineering and Design, Vol. 150, pp. 215-223, (1994). Schwer, L.E., “Demonstration of the Continuous Surface Cap Model with Damage: Concrete Unconfined Compression Test Calibration,” LS-DYNA Geomaterial Modeling Short Course Notes, July (2001). Schwer, L.E., W. Cheva, and J.O. Hallquist, “A Simple Viscoelastic Model for Energy Absorbers Used in Vehicle-Barrier Impact,” in Computation Aspects of Contact, Impact, and Penetration, Edited by R.F. Kulak and L.E. Schwer, Elmepress International, Lausanne, Switzerland, pp. 99-117 (1991). Schwer, L.E. and Y.D. Murray, “A Three-Invariant Smooth Cap Model with Mixed in for Numerical and Analytical Methods Hardening,” International Journal Geomechanics, Volume 18, pp. 657-688, (1994). Seeger, F., M. Feucht, T. Frank (DaimlerChrysler AG), and A. Haufe, B. Keding (DYNAmore GmbH), “An Investigation on Spotweld Modeling for Crash Simulation with LS-DYNA”, 4th LS-DYNA-Forum, Bamburg, Germany, October (2005), ISBN 3-9809901-1-7. Shi, M.F., and Gelisse, S., “Issues on the AHSS Forming Limit Determination”, International Deep Drawing Research Group (IDDRG), Porto, Portugal, June, 2006. Shi, M.F., Zhu, X.H., Xia, C., and Stoughton T., “Determination of Nonlinear Isotropic/Kinematic Hardening Constitutive Parameter for AHSS using Tension and Compression Tests”, p. 137-142, Proceedings of the 7th International Conference and Workshop on Numerical Simulation of 3D Sheet Metal Forming Processes (NUMISHEET 2008), Interlaken, Switzerland, September, 2008. Sheppard, S.D., Estimations of Fatigue Propagation Life in Resistance Spot Welds, ASTM STP 1211, pp. 169-185, (1993). Sheppard, T. and Wright, D.S., “Determination of flow stress: Part 1 constitutive equation for aluminum alloys at elevated temperatures”, Metals Technology, p. 215, June 1979. Shvets, I.T. and Dyban, E., P., “Contact Heat Transfer between Plane Metal Surfaces”, Int. Chem. Eng., Vol. 4, No. 4, 621 (1964). Simo, J.C., J.W. Ju, K.S. Pister, and R.L. Taylor, “An Assessment of the Cap Model: Consistent Return Algorithms and Rate-Dependent Extension,” J. Eng. Mech., Vol. 114, No. 2, 191-218 (1988a). REFERENCES Simo, J.C., J.W. Ju, K.S. Pister, and R.L. Taylor, “Softening Response, Completeness Condition, and Numerical Algorithms for the Cap Model,” Int. J. Numer. Analy. Meth. Eng., (in press) (1988b). Simo, J. C., J.W. Ju, K.S. Pister, and R.L. Taylor, “Softening Response, Completeness Condition, and Numerical Algorithms for the Cap Model,” Int. J. Numer. Analy. Meth. Eng. (1990). Solberg, J.M., and C.M. Noble, “Contact Algorithm for Small-Scale Surface Features with Application to Finite Element Analysis of Concrete Arch Dams with Beveled Contraction Joints”, Lawrence Livermore National Laboratory (2002). Spanos, P.D. and Tsavachidis, S., “Deterministic and stochastic analyses of a nonlinear system with a Biot visco-elastic element,” Earthquake Engineering and Structural Dynamics, vol. 30, pp. 595–612, (2001). Steinberg, D.J. and M.W. Guinan, A High-Strain-Rate Constitutive Model for Metals, University of California, Lawrence Livermore National Laboratory, Rept. UCRL- 80465 (1978). Steinberg, D.J. and C.M. Lund, “A Constitutive Model for Strain Rates form 10-4 to 106 S-1,” J. Appl. Phys., 65, p. 1528 (1989). Stillman, D.W. and J.O. Hallquist, INGRID: A Three-Dimensional Mesh Generator for Modeling Nonlinear Systems, University of California, Lawrence Livermore National Laboratory, Rept. UCID-20506. (1985). Stojko, S., privated communication, NNC Limited, Engineering Development Center (1990). Stahlecker Z., Mobasher B., Rajan S.D., Pereira J.M., “Development of reliable modeling methodologies for engine fan blade out containment analysis. Part II: Finite element analysis”, International Journal of Impact Engineering, Volume 36, Issue 3, Pages 447-459, (2009) Storakers, B., “On material representation and constitutive branching in finite compressible elasticity”, J. Mech. Phy. Solids, 34 No. 2, 125-145 (1986). Stouffer and Dame, Inelastic Deformation of Metals, Wiley, (1996). Stout, M.G., D.E. Helling, T.L. Martin, and G.R. Canova, Int. J. Plasticity, Vol. 1, pp. 163-174, (1985). Structural Engineers Association of California, Tentative Lateral Force Requirements, Seismology Committee, SEAOC, 1974, 1990, 1996. REFERENCES Sussman, T. and Bathe, K.J., “A Finite Element Formulation for Nonlinear Incompressible Elastic and Inelastic Analysis,” Computers & Structures, 26, Number 1/2, 357-409 (1987). Tabiei, A. and I. Ivanov, “Computational micro-mechanical Model of Flexible Woven Fabric for Finite Element Impact Simulation,” IJNME, 53, (6), 1259-1276, (2002). Tahoe User Guide, Sandia National Laboratory, can be downloaded from: www.sandia.gov, Input version 3.4.1, (2003). Taylor, L.M. and D.P. Flanagan, PRONTO3D A Three-Dimensional Transient Solid Dynamics Program, Sandia Report: SAND87-1912, UC-32, (1989). Taylor, R.L. Finite element analysis of linear shell problems, in Whiteman, J.R. (ed.), Proceedings of the Mathematics in Finite Elements and Applications, Academic Press, New York, 191-203, (1987). Taylor, R.L. and Simo, J.C. Bending and membrane elements for the analysis of thick and thin shells, Proc. of NUMETA Conference, Swansea (1985). Tsai, S.W. and E.M. Wu, “A General Theory of Strength for Anisotropic Materials,” J. Composite Materials, 5, pp. 73-96 (1971). Tuler, F.R. and B.M. Butcher, “A Criterion for the Time Dependence of Dynamic Fracture,” The International Journal of Fracture Mechanics, Vol. 4, No. 4, (1968). Tvergaard, V. and J.W. Hutchinson, “The relation between crack growth resistance and fracture process parameters in elastic-plastic solids,” J. of the Mech. And Phy. of Solids, 40, pp1377-1397, (1992) Tvergaard, V. and Needleman, A., “Analysis of the cup-cone fracture in a round tensile bar”, Acta Metallurgica, 32, 157-169 (1984). Vawter, D., “A Finite Element Model for Macroscopic Deformation of the Lung,” published in the Journal of Biomechanical Engineering, Vol.102, pp. 1-7 (1980). VDA Richtlinier (Surface Interfaces), Version 20, Verband der Automobilindustrie e.v., Frankfurt, Main, Germany, (1987). Vegter, H., Horn, C.H.L.J. ten, An, Y., Atzema, E.H., Pijlman, H.H., Boogaard, A.H. van den, Huetink, H., “Characterisation and Modelling of the Plastic Material Behaviour and its Application in Sheet Metal Forming Simulation”, Proceedings of 7th International Conference on Computational Plasticity COMPLAS VII, Barcelona (2003). REFERENCES Vegter, H., and Boogaard, A.H. van den, “A plane stress yield function for anisotropic sheet material by interpolation of biaxial stress states”, International Journal of Plasticity 22, 557-580 (2006). Walker, J.C., Ratcliffe M.B., Zhang P., Wallace A.W., Fata, B., Hsu E., Saloner D., and Guccione J.M. “MRI-based finite-element analysis of left ventricular aneurysm”, Am J Physiol Heart Circ Physiol 289(2): H692:700 (2005). Wang, J.T. and O.J. Nefske, “A New CAL3D Airbag Inflation Model,” SAE paper 880654, 1988. Wang, J.T., “An Analytical Model for an Airbag with a Hybrid Inflator”, Publication R&D 8332, General Motors Development Center, Warren, Mi. (1995). Wang, J.T., “An Analytical Model for an Airbag with a Hybrid Inflator”, AMD-Vol. 210, BED-Vol. 30, ASME, pp 467-497, (1995). Wang, K., Y. J. Chao, Y. J., X. Zhu., and K.W. Miller “Dynamic Separation of Resistance Spot Welded Joints: Part II—Analysis of Test Results and a Model” Exp Mech Vol 50, Issue 7, pp 901-913 (2010). Weiss, J.A., Maker, B.N. and Govindjee, S., “Finite Element Implementation of Incompressible, Transversely Isotropic Hyperelasticity”, Comp. Meth. Appl. Mech. Eng., 135, 107-128 (1996). Wen, T.K. “Method for Random Vibration of Hysteretic Systems”, J. Engrg. Mech., ASCE, Vol. 102, No. EM2, Proc. Paper 12073, pp.249-263 (1976). Whirley, R. G., and J. O. Hallquist, DYNA3D, A Nonlinear, Explicit, Three- Dimensional Finite Element Code for Solid and Structural Mechanics-Users Manual, Report No.UCRL-MA-107254 , Lawrence Livermore National Laboratory, (1991). Whirley, R. G., and G.A. Henshall, “Creep Deformation Structural Analysis Using An Efficient Numerical Algorithm,” IJNME, Vol. 35, pp. 1427-1442, (1992). Wilkins, M.L., “Calculations of Elastic Plastic Flow,” Meth. Comp. Phys., 3, (Academic Press), 211-263 (1964). Wilkins, M.L., Calculation of Elastic-Plastic Flow, University of California, Lawrence Livermore National Laboratory, Rept. UCRL-7322, Rev. I (1969). Wilkins, M.L., The Use of Artificial Viscosity in Multidimensional Fluid Dynamics Calculations, University of California, Lawrence Livermore National Laboratory, Rept. UCRL-78348 (1976) REFERENCES Wilkins, M.L., R.E. Blum, E. Cronshagen, and P. Grantham, A Method for Computer Simulation of Problems in Solid Mechanics and Gas Dynamics in Three Dimensions and Time, University of California, Lawrence Livermore National Laboratory, Rept. UCRL-51574 (1974). Wilkins, M.L., J.E. Reaugh, B. Moran, J.K. Scudder, D.F. Quinones, M.E. Prado, Fundamental Study of Crack Initiation and Propagation Annual Progress Report, Report UCRL-52296, Lawrence Livermore National Laboratory, Livermore, CA. (1977). Wilkins, M.L, Streit, R.D, and Reaugh, J.E. Cumulative-Strain-Damage Model of Ductile Fracture: Simulation and Prediction of Engineering Fracture Tests, Report UCRL- 53058, Lawrence Livermore National Laboritory, Livermore, CA (1980). Williams K. V., Vaziri R., Poursartip A., “A Physically Based Continuum Damage Mechanics Model for Thin Laminated Composite Structures.” Int J Solids Struct, Vol 40(9), 2267-2300 Wilson, E.L. Three Dimensional Static and Dynamic Analysis of Structures, Computers and Structures, Inc., Berkeley CA, (2000). Winters, J.M., “Hill-based muscle models: A systems engineering perspective,” In Multiple Muscle Systems: Biomechanics and Movement Organization, JM Winters and SL-Y Woo eds, Springer-Verlag (1990). Winters J.M. and Stark L., “Estimated mechanical properties of synergistic muscles involved in movements of a variety of human joints,” J Biomechanics 21:1027- 1042, (1988). Woodruff, J.P., KOVEC User's Manual, University of California, Lawrence Livermore National Laboratory, Report UCRL-51079, (1973). Worswick, M.J., and Xavier Lalbin, Private communication, Livermore, California, (1999). Wu Y., John E. Crawford, Shengrui Lan, and Joseph M., “Validation studies for concrete constitutive models with blast test data”, 13th International LS-DYNA User’s Conference, Dearborn MI, (2014). Xia, Q.S., M.C. Boyce, and D.M. Parks, “A constitutive model for the anisotropic elasticplastic deformation of paper and paperboard,” Int. J. Solids and Struct., 39, 4053-4071 (2002). Yamasaki, H., M. Ogura, R. Nishimura, and K. Nakamura, “Development of Material Model for Crack Propagation of Casting Aluminum”, Presented at the 2006 JSAE Annual Congress, Paper Number 20065077, (2006). REFERENCES Yen, C.F., “Ballistic Impact Modeling of Composite Materials”, Proceedings of the 7th International LS-DYNA Users Conference, Dearborn, MI, May 19-21, 2002, 6.15- 6.25. Yoshida, F. and Uemori, T., “A Model of Large-Strain Cyclic Plasticity Describing the Bauschinger Effect and Work Hardening Stagnation”, International Journal of Plasticity 18, 661-686 (2002). Yoshida, F. and Uemori, T., “A Model of Large-Strain Cyclic Plasticity and its Application to Springback Simulation”, International Journal of Mechanical Sciences, Vol. 45, 1687-1702, (2003). Zajac F.E., “Muscle and tendon: Properties, models, scaling, and application to biomechanics and motor control”, CRC Critical Reviews in Biomedical Engineering 17(4):359-411, (1989). Zayas, V.A., Low, S.S. and Mahin, S.A., “A Simple Pendulum Technique for Achieving Seismic Isolation”, J. Earthquake Spectra, Vol. 6, No. 2, pp. 317-334 (1990). Zhang, S., Approximate Stress Intensity Factors and Notch Stresses for Common Spot- Welded Specimens, Welding Research Supplement, pp. 173s-179s, (1999). Zhang, S., McCormick, P.G., Estrin, Y., “The morphology of Portevin-Le Chatelier bands: Finite element simulation for Al-Mg-Si”, Acta Materialia 49, 1087-1094, (2001). APPENDIX A APPENDIX A: User Defined Materials Getting Started with User Defined Features As a way of entering the topic, we begin by giving a general introduction to User Defined Features (UDF) in general. This section is supposed to be valid for any UDF described in the remaining appendices and serves as a practical guide to get to the point where technical coding may commence. For a comprehensive overview of UDFs and its applications, please refer to Erhart [2010] which can be seen as a complement to the present text. Object version lsdyna_...tgz lsdyna ...zip Unpacking to usermat Compiler (external) Intel Fortran (IFC) Portland Groups (PGI) GNU (for shared libs and modules) Libraries libdyna.a libmf2.a etc Includes nhisparm.inc memaia.inc etc Source dyn21.F dyn21b.F etc Makefile Download The first thing to do is to download an object version of LS-DYNA for the computer architecture/platform of interest. This is a compressed package (.tgz,.tar.gz,.zip) provided by your local LS-DYNA distributor whose unpacked content is not only a single binary executable but a usermat directory possibly including •precompiled static object libraries (.a, .lib) •fortran source code files (.f, .F) •include files (.inc) •makefile It is important to know what version to download, i.e., a version that is compatible with your computer environment in terms of architecture, operating system and possible MPI implementation in case of MPP. This may not be obvious to all users and for questions regarding this we refer to your LS-DYNA distributor. An object version does not require a special license but goes under the general LS-DYNA license agreement. The picture above gives a conceptual overview of the usermat package, and at this point APPENDIX A we need to mention that presence of libraries and include files are made obsolete with the advent of modules as to be explained below, but we start with the non-modular approach. Static or Dynamic linking To get something that is actually runnable it is necessary to compile the source code files and link the resulting object files either to a shared object (.so, .dll) or with the precompiled libraries to a binary executable. The former option requires a shared object version of the usermat package while the latter assumes a statically linked version, and this is thus a choice that needs to be made before retrieving the package. Working with shared objects is more flexible in the sense that a binary executable can be installed once and for all and the (small) shared object is dynamically linked at runtime as a plugin. Upon execution, LS-DYNA will look for the shared object file in directories specified by a library path that is usually set/edited in the run command script, and when found the shared object content is linked to the execution. On Linux OS’s this is for instance governed by the environment variable LD_LIBRARY_PATH. The shared object is easily substituted or the run command script can be edited to redirect the location of the shared object, and this facilitates portability when working on large projects. A statically linked version requires that the entire binary executable is generated at compile time and this option may be preferred if working on small projects or during the development phase. Compiler and Compiling The compilation is usually performed in the usermat (working) directory using a terminal window. The object version does not contain a compiler but it is assumed that the appropriate compiler is installed on your system and accessible from your working directory. To render compatibility between the precompiled libraries or binary executable and your compiled object files, the appropriate compiler is the (by LSTC) designated compiler with which the precompiled libraries or binary are readily compiled. As examples, on Linux this is typically either the Intel Fortran Compiler (IFC) on Red Hat or CentOS or Portland Groups Compiler (PGF) on SUSE, and on Windows it is the Intel Fortran Compiler (IFC) in combination with Microsoft Visual Studio (MSVS). For MPP you also need a wrapper for whatever MPI implementation you have installed, but again, consult your LS-DYNA distributor for detailed information. To compile, execute ‘make’ in the terminal window and in most cases this will generate a shared object or binary executable depending on your type of LS-DYNA object version, and if not it comes down to interpreting error messages. A possible reason for failure is that the makefile that comes with the usermat package does not contain appropriate compiler directives and requires some editing. This could range from trivial tasks like altering the path used to actually find the compiler on your system to more complex endeavors such as adding or changing compiler flags. An even worse scenario is that your operating system is not up-to-date and may require that the library content on your computer is somehow updated. Whatever the reason might be, any APPENDIX A case is unique and the situation is preferrably resolved by your computer administrator in collaboration with your LS-DYNA distributor. Execution When compiling a virgin instance of an object version, the generated executable {xyz}dyna in combination with a possible shared object lib{xyz}dyna_{t}_{Y}.{Z}.so makes up an exact replica of a non-object executable counterpart. It is only when the source code is modified that a customized version is generated. In the adopted binary and shared object naming convention above, xyz stands for smp or mpp, t is either s for single precision or d for double precision, Y is the base revision number for the LS-DYNA and Z is the corresponding release revision number. Z is always larger than Y. The binary and shared object may be left in the working directory, moved to some other location on your system or properly installed for execution on clusters by a queuing system. Obviously the way execution is performed is affected accordingly, and we don’t claim to cover all these situations but leave this task to you and your computer administrator. While the executable may be renamed, a shared object should in general not be since this dynamic dependence is built into the executable. During the development phase it may be convenient to leave the binary in its place to facilitate debugging, but possibly move the shared object to the execution directory to not having to edit the library path for the executable to find it. Two Linux examples on how to run an input file are given in the following, one assuming an SMP static object version has been downloaded and the other an MPP shared object version. Let /path_to_my_source/usermat be the complete path to the working directory and in.k be the name of the LS-DYNA keyword input file. If located in the execution directory, i.e., the directory containing in.k, the problem is run as /path_to_my_source/usermat/lsdyna i = in.k in the SMP case. For the MPP shared object case, you may copy the shared object file to the execution directory which is a default directory for executables to look for dynamic object files. Assuming the MPI software is platform-MPI, the input file could be run on 2 cores as /path_to_platform-mpi/bin/mpirun –np 2 /path_to_my_source/usermat/mppdyna i = in.k These two examples are only intended to indicate how to treat the compiled files and changes in details thereof are to be expected. Coding All subroutines for the UDFs are collected in the files dyn21.f and dyn21b.f and are ready for editing using your favorite text editor. Mechanical user materials, user defined loading, user defined wear and friction are contained in dyn21.f, while user defined elements and thermal user materials are in dyn21b.f, just to give a few examples. The prevailing programming language is Fortran 77, but many compilers support Fortran 90 APPENDIX A and it may also be possible to write C code but this requires some manipulation of the makefile and function interfaces. Each individual feature is connected to one or a few keywords to properly take advantage of innovative coding. For user materials, this keyword is *MAT_USER_DEFINED_MATERIAL_MODELS and is described in detail below, and for user defined loads the corresponding keyword is *USER_LOADING. We refer to the individual keyword sections for details on their respective usage. Module Concept As of version R9 of LS-DYNA, there is yet another way of approaching user defined features, namely through the concept of modules. The purpose is twofold; 1.To facilitate working with UDFs in that the content of the usermat package is significantly reduced and instead replaced by *MODULE keywords 2.To enhance flexibility when incorporating features delivered as shared objects by third parties By way of 1, the usermat package only consists of a makefile and a few source code files, and in principle all the user needs to do is to (i) implement the feature of interest in the source code files, (ii) compile to a shared object using the makefile, and (iii) use the keyword input file to access the generated object. A shared object to be used in this way is henceforth called a module. One of two nice side effects coming out of this approach is that the restriction on the choice of compiler is alleviated, the source code files can be compiled with any valid fortran compiler as long as the generated module is linkable as a plug-in to LS-DYNA. The other is that a standard LS-DYNA executable can be used to access the modules, i.e., it is not required to acquire a special “module” version to use with this approach. To explain how LS-DYNA in practice access modulus and specific routines therein, and at the same time address 2 above, the *MODULE keyword requires some attention by means of an example. APPENDIX A module usermat package LS-DYNA standard executable, smp or mpp Source edit to create feature Makefile for compiling Compiler (external) non-commercial is ok *KEYWORD … *MODULE … Compilie to module my_object.so subroutine your_object.so subroutine Module provided by In a standard version of LS-DYNA the keywords *MODULE_PATH *MODULE_LOAD *MODULE_USE are available, see the Section on *MODULE for further explanations than what is provided here. With reference to the picture above, we assume that my_object.so and your_object.so are two independently generated modules, and both are located in directory /path_to_modules. We also assume that these two objects contain the same routines names, one of them being the source code for user material 41 (subroutine umat41). Without the present approach, it would be at least intricate to execute both of these two source codes in the same LS-DYNA executable and same keyword input. A simple way of dealing with this here is to use the following set of keywords *MODULE_PATH /path_to_modules *MODULE_LOAD $ MDLID TITLE myid my library $ FILENAME my_object.so *MODULE_LOAD $ MDLID TITLE yourid your library $ FILENAME your_object.so *MODULE_USE $ MDLID APPENDIX A myid $ TYPE PARAM1 PARAM2 UMAT 1001 41 *MODULE_USE $ MDLID yourid $ TYPE PARAM1 PARAM2 UMAT 1002 41 *MAT_USER_DEFINED_MATERIAL_MODELS $ MID RO MT 1 7.85e-9 1001 … *MAT_USER_DEFINED_MATERIAL_MODELS $ MID RO MT 2 7.85e-9 1002 … *PART first part $ PID SECID MID 1 1 1 *PART second part $ PID SECID MID 2 2 2 The *MODULE_PATH lists the path(s) to the modules to be loaded, *MODULE_LOAD actually loads the module into LS-DYNA, and *MODULE_USE tells LS-DYNA how to access routines in the module. In this particular example, the rules (TYPE = UMAT) are that a user material *MAT_USER_... with MT set to 1001 (because PARAM1 = 1001) will execute subroutine umat41 (because PARAM2 = 41) in the module with id myid (because MDLID = myid) and in the same manner user material with MT set to 1002 will also execute subroutine umat41 but now in the module with id yourid. Hence we have made part 1 and part 2, in the same keyword input file, execute the same subroutine (by name) but in different modules. Obviously this generalizes to any number of modules by analogy, see *MODULE_USE for many more rules and yet another example. General overview We now turn to the specific documentation of user defined materials. Up to ten user subroutines can currently be implemented simultaneously to update the stresses in solids, shells, beams, discrete beams and truss beams. This text serves as an introductory guide to implement such a model. Note that names of variables and subroutines below may differ from the actual ones depending on platform and current version of LS-DYNA. When the keyword *MAT_USER_DEFINED_MATERIAL_MODELS is defined for a part in the keyword deck, LS-DYNA calls the subroutine usrmat with appropriate input data APPENDIX A for the constitutive update. This routine in turn calls urmathn for 2D and 3D solid elements, urmats for 2D plane stress and 3D shell elements, urmatb for beam elements, urmatd for discrete beam elements and urmatt for truss beam elements. In these routines, which may be modified by the user if necessary, the following data structures are initialized for the purpose of being supplied to a specific scalar material subroutine. sig(6) – stresses in previous time step eps(6) – strain increments epsp – effective plastic strain in previous time step hsv(*) – history variables in previous time step excluding plastic strain dt1 – current time step size temper - current temperature failel – flag indicating failure of element If the vectorization flag is active (IVECT = 1) on the material card, variables are in general stored in vector blocks of length nlq, with vector indexes ranging from lft to llt , which allows for a more efficient execution of the material routine. As an example, the data structures mentioned above are for the vectorized case exchanged for sigX(nlq) – stresses in previous time step dX(nlq) – strain increments epsps(nlq) – effective plastic strains in previous time step hsvs(nlq,*) – history variables in previous time step dt1siz(nlq) - current time step sizes temps(nlq) – current temperatures failels(nlq) – flags indicating failure of elements where X ranges from 1 to 6 for the different components. Each entry in a vector block is associated with an element in the finite element mesh for a fix integration point. The number of entries in the history variables array (indicated by * in the above) matches the number of history variables requested on the material card (NHV). Hence the number NHV should equal to the number of history variables excluding the effective plastic strain since this variable is given a special treatment. All history variables, including the effective plastic strain, are initially zero. Furthermore, all user-defined material models require a bulk modulus and shear modulus for transmitting boundaries, contact interfaces, rigid body constraints, and time step calculations. This generally means that the length of material constants array LMC must be increased by 2 for the storage of these parameters. In addition to the variables mentioned above, the following data can be supplied to the user material routines, regardless of whether vectorization is used or not. cm(*) – material constants array capa – transverse shear correction factor for shell elements tt – current time APPENDIX A crv(lq1,2,*) – array representation of curves defined in the keyword deck A specific material routine, umatXX in the scalar case or umatXXv in the vector case, is now called with any necessary parameters of the ones above, and possibly others as well. The letters XX stands for a number between 41 and 50 and matches the number MT on the material card. This subroutine is written by the user, and should update the stresses and history variables to the current time. For shells and beams it is also necessary to determine the strain increments in the directions of constrained zero stress. To be able to write different stress updates for different elements, the following character string is passed to the user-defined subroutine etype – character string that equals solid, shell, beam, dbeam or tbeam A sample user subroutine of a hypo-elastic material in the scalar case is provided below. This sample and the others below are from the dyn21.F file that is distributed with version R6.1. Sample user subroutine 41 subroutine umat41 (cm,eps,sig,epsp,hsv,dt1,capa,etype,tt, 1 temper,failel,crv,nnpcrv,cma,qmat,elsiz,idele,reject) c c****************************************************************** c| Livermore Software Technology Corporation (LSTC) | c| ------------------------------------------------------------ | c| Copyright 1987-2008 Livermore Software Tech. Corp | c| All rights reserved | c****************************************************************** c c isotropic elastic material (sample user subroutine) c c Variables c c cm(1)=first material constant, here young's modulus c cm(2)=second material constant, here poisson's ratio c . c . c . c cm(n)=nth material constant c c eps(1)=local x strain increment c eps(2)=local y strain increment c eps(3)=local z strain increment c eps(4)=local xy strain increment c eps(5)=local yz strain increment c eps(6)=local zx strain increment c c sig(1)=local x stress c sig(2)=local y stress c sig(3)=local z stress c sig(4)=local xy stress c sig(5)=local yz stress c sig(6)=local zx stress c c hsv(1)=1st history variable APPENDIX A c hsv(2)=2nd history variable c . c . c . c . c hsv(n)=nth history variable c c dt1=current time step size c capa=reduction factor for transverse shear c etype: c eq."solid" for solid elements c eq."sld2d" for shell forms 13, 14, and 15 (2D solids) c eq."shl_t" for shell forms 25, 26, and 27 (shells with thickness c stretch) c eq."shell" for all other shell elements plus thick shell forms 1 c and 2 c eq."tshel" for thick shell forms 3 and 5 c eq."hbeam" for beam element forms 1 and 11 c eq."tbeam" for beam element form 3 (truss) c eq."dbeam" for beam element form 6 (discrete) c eq."beam " for all other beam elements c c tt=current problem time. c c temper=current temperature c c failel=flag for failure, set to .true. to fail an integration point, c if .true. on input the integration point has failed earlier c c crv=array representation of curves in keyword deck c c nnpcrv=# of discretization points per crv() c c cma=additional memory for material data defined by LMCA at c 6th field of 2nd crad of *DATA_USER_DEFINED c c elsiz=characteristic element size c c idele=element id c c reject (implicit only) = set to .true. if this implicit iterate is c to be rejected for some reason c c All transformations into the element local system are c performed prior to entering this subroutine. Transformations c back to the global system are performed after exiting this c routine. c c All history variables are initialized to zero in the input c phase. Initialization of history variables to nonzero values c may be done during the first call to this subroutine for each c element. c c Energy calculations for the dyna3d energy balance are done c outside this subroutine. c include 'nlqparm' include 'bk06.inc' include 'iounits.inc' dimension cm(*),eps(*),sig(*),hsv(*),crv(lq1,2,*),cma(*) integer nnpcrv(*) logical failel,reject character*5 etype c if (ncycle.eq.1) then if (cm(16).ne.1234567) then APPENDIX A call usermsg('mat41') endif endif c c compute shear modulus, g c g2 =abs(cm(1))/(1.+cm(2)) g =.5*g2 c if (etype.eq.'solid'.or.etype.eq.'shl_t'.or. 1 etype.eq.'sld2d'.or.etype.eq.'tshel') then if (cm(16).eq.1234567) then call mitfail3d(cm,eps,sig,epsp,hsv,dt1,capa,failel,tt,crv) else if (.not.failel) then davg=(-eps(1)-eps(2)-eps(3))/3. p=-davg*abs(cm(1))/(1.-2.*cm(2)) sig(1)=sig(1)+p+g2*(eps(1)+davg) sig(2)=sig(2)+p+g2*(eps(2)+davg) sig(3)=sig(3)+p+g2*(eps(3)+davg) sig(4)=sig(4)+g*eps(4) sig(5)=sig(5)+g*eps(5) sig(6)=sig(6)+g*eps(6) if (cm(1).lt.0.) then if (sig(1).gt.cm(5)) failel=.true. endif endif end if c else if (etype.eq.'shell') then if (cm(16).eq.1234567) then call mitfailure(cm,eps,sig,epsp,hsv,dt1,capa,failel,tt,crv) else if (.not.failel) then gc =capa*g q1 =abs(cm(1))*cm(2)/((1.0+cm(2))*(1.0-2.0*cm(2))) q3 =1./(q1+g2) eps(3)=-q1*(eps(1)+eps(2))*q3 davg =(-eps(1)-eps(2)-eps(3))/3. p =-davg*abs(cm(1))/(1.-2.*cm(2)) sig(1)=sig(1)+p+g2*(eps(1)+davg) sig(2)=sig(2)+p+g2*(eps(2)+davg) sig(3)=0.0 sig(4)=sig(4)+g *eps(4) sig(5)=sig(5)+gc*eps(5) sig(6)=sig(6)+gc*eps(6) if (cm(1).lt.0.) then if (sig(1).gt.cm(5)) failel=.true. endif endif end if elseif (etype.eq.'beam ' ) then q1 =cm(1)*cm(2)/((1.0+cm(2))*(1.0-2.0*cm(2))) q3 =q1+2.0*g gc =capa*g deti =1./(q3*q3-q1*q1) c22i = q3*deti c23i =-q1*deti fac =(c22i+c23i)*q1 eps(2)=-eps(1)*fac-sig(2)*c22i-sig(3)*c23i eps(3)=-eps(1)*fac-sig(2)*c23i-sig(3)*c22i davg =(-eps(1)-eps(2)-eps(3))/3. p =-davg*cm(1)/(1.-2.*cm(2)) sig(1)=sig(1)+p+g2*(eps(1)+davg) sig(2)=0.0 sig(3)=0.0 APPENDIX A sig(4)=sig(4)+gc*eps(4) sig(5)=0.0 sig(6)=sig(6)+gc*eps(6) c elseif (etype.eq.'tbeam') then q1 =cm(1)*cm(2)/((1.0+cm(2))*(1.0-2.0*cm(2))) q3 =q1+2.0*g deti =1./(q3*q3-q1*q1) c22i = q3*deti c23i =-q1*deti fac =(c22i+c23i)*q1 eps(2)=-eps(1)*fac eps(3)=-eps(1)*fac davg =(-eps(1)-eps(2)-eps(3))/3. p =-davg*cm(1)/(1.-2.*cm(2)) sig(1)=sig(1)+p+g2*(eps(1)+davg) sig(2)=0.0 sig(3)=0.0 c else c write(iotty,10) etype c write(iohsp,10) etype c write(iomsg,10) etype c call adios(TC_ERROR) cerdat(1)=etype call lsmsg(3,MSG_SOL+1150,ioall,ierdat,rerdat,cerdat,0) endif c c10 format(/ c 1 ' *** Error element type ',a,' can not be', c 2 ' run with the current material model.') return end Based on the subroutine umat41 shown above, the following material input… *MAT_USER_DEFINED_MATERIAL_MODELS $# mid ro mt lmc nhv iortho ibulk ig 1 7.8300E-6 41 4 0 0 3 4 $# ivect ifail itherm ihyper ieos 0 0 0 0 0 $ E PR BULK G $# p1 p2 p3 p4 p5 p6 p7 p8 2.000000 0.300000 1.667000 0.769200 0.000 0.000 0.000 0.000 … is functionally equivalent to … *MAT_ELASTIC $# mid ro e pr da db not used 1 7.8300E-6 2.000000 0.300000 0.000 0.000 0 APPENDIX A Load curves and tables ADDITIONAL FEATURES If the material of interest should require load curves, for instance a curve defining yield stress as a function of effective plastic strain, curve and table lookup are easily obtained by predefined routines. The routines to be called are subroutine crvval(crv,nnpcrv,eid,xval,yval,slope) and subroutine crvval_v(crv,nnpcrv,eid,xval,yval,slope,lft,llt) where the former routine is used in the scalar context and the latter for vectorized umat. The arguments are the following crv - the load curve array (available in material routine, just pass on) nnpcrv - curve data pointer (available in material routine, just pass on) eid - external load curve ID, i.e., the load curve ID taken from the keyword deck .GT.0: Use approximate representation of curve .LT.0: Use exact representation of curve (with id –eid) xval - abscissa value yval - ordinate value (output from routine) slope - slope of curve (output from routine) lft - first index of vector llt - final index of vector where xval, yval and slope are scalars in the scalar routine and vectors of length nlq in the vectorized routine. Note that eid should be passed as float. Using a positive number for eid will use the approximative representation of the curve, whereas if eid is a negative number the extraction will be made on the curve as it is defined in the keyword input deck. For tables, two subroutines are available for extracting values. A scalar version is subroutine tabval(crv,nnpcrv,eid,dxval,yval,dslope,xval,slope) and a vector version is subroutine 1 tabval_v(crv,nnpcrv,eid,dxval,yval,dslope,lft,llt,xval,slope) where crv - curve array (available in material routine, just pass on) nnpcrv - curve pointer (available in material routine, just pass on) APPENDIX A eid - external table id (data type real), i.e., table id taken from keyword deck GT.0: Use approximative representation of curve LT.0: Use exact representation of curve (with id –eid) dxval - abscissa value (x2-axis) yval - ordinate value (y-axis, output from routine) dslope - slope of curve (dy/dx2, output from routine) xval - abscissa value (x1-axis) slope - slope of curve (dy/dx1, output from routine) lft - vector index llt - vector index In the scalar routine, dxval, yval, dslope, xval and slope are all scalars whereas in the vector routine they are vectors of length nlq. Also here, using a positive number for eid will use the approximative representation of the table, whereas if eid is a negative number the extraction will be made on the table as it is defined in the keyword input deck. Local coordinate system If the material model has directional properties, such as composites and anisotropic plasticity models, the local coordinate system option can be invoked. This is done by putting IORTHO equal to 1 on the material card. This also requires two additional cards with values for how the coordinate system is formed and updated. When this option is used, all data passed to the constitutive routine umatXX or umatXXv is in the local system and the transformation back to the global system is done outside this user- defined routine. There is one exception however, see the section on the deformation gradient. Temperature For a material with thermal properties, temperatures are made available by putting the flag ITHERMAL equal to 1 on the material card. The temperatures in the elements are then available in the temper variable for a scalar and temps array for the vectorized implementation. For a coupled thermal structural analysis, the thermal problem is solved first and temperatures at the current time are available in the user-defined subroutine. Calculation of dissipated heat in the presence of plastic deformation is taken care of by LS-DYNA and needs not be considered by the user. If the time derivative of the temperature is needed for the stress update, a history variable that contains the temperature in the previous time step should be requested. The time derivative can then be obtained by a backward finite difference estimate. APPENDIX A Failure It is possible to include failure in the material model, resulting in the deletion of elements that fulfill a certain failure criterion. To accomplish this, the flag IFAIL must be set to 1 or a negative number on the material card. For a scalar implementation, the variable failel is set to .true. when a failure criterion is met. For a vectorized implementation, the corresponding entry in the failels array is set to .true. Deformation gradient For some materials, the stresses are not obtained from incremental strains, but are expressed in terms of the deformation gradient 𝐅. This is the case for hyper-elastic(- plastic) materials. To make the deformation gradient available for bricks and shells in the user-defined material subroutines, the variable IHYPER on the material card should be set to 1. The deformation gradient components 𝐹11, 𝐹21, 𝐹31, 𝐹12, 𝐹22, 𝐹32, 𝐹13, 𝐹23 and 𝐹33can then be found in the history variables array in positions NHV+1 to NHV+9, i.e., the positions coming right after the requested number of history variables. For shell elements, the components of the deformation gradient are with respect to the co-rotational system for the element currently used. In this case the third row of the deformation gradient, i.e., the components 𝐹31, 𝐹32 and 𝐹33, will not be properly updated when entering the user-defined material routine. These components depend on the thickness strain increment which in turn must be determined so that the normal stress in the shell vanishes. For a given thickness strain increment d3, these three components, f31, f32 and f33, can be determined by calling the subroutine subroutine compute_f3s(f31,f32,f33,d3) for a scalar implementation and subroutine compute_f3(f31,f32,f33,d3,lft,llt) for a vector implementation. The first four arguments are arrays of length nlq for the vector routine and scalars for the scalar routine. For hyper-elastic materials there are push forward operations that can be called from within the user defined subroutines. These are subroutine push_forward_2(sig1,sig2,sig3,sig4,sig5,sig6, f11,f21,f31,f12,f22,f32,f13,f23,f33,lft,llt) which performs a push forward operation on the stress tensor, and the corresponding scalar routine subroutine push_forward_2s(sig1,sig2,sig3,sig4,sig5,sig6, f11,f21,f31,f12,f22,f32,f13,f23,f33) In the latter subroutine all arguments are scalars whereas the corresponding entries in the vectorized routine are vectors of length nlq. The sig1 to sig6 are components of the stress tensor and f11 to f33 are components of the deformation gradient. APPENDIX A If the local coordinate system option is invoked (IORTHO = 1), then the deformation gradient is transformed to this local system prior to entering the user-defined material routine according to 𝑠 𝐹𝑘𝑗 𝑠 refers to a transformation between the current global and material frames. where 𝑄𝑖𝑗 For IORTHO equal to 1 one can choose to put IHYPER equal to –1 which results in that the deformation gradient is transformed according to 𝐹̅𝑖𝑗 = 𝑄𝑘𝑖 𝑟 𝐹̅𝑖𝑗 = 𝐹𝑖𝑘𝑄𝑘𝑗 𝑟 is the transformation between the reference global and material and frames. where 𝑄𝑖𝑗 For this latter option the spatial frame remains the global one so the stresses should be expressed in this frame of reference upon exiting the user defined routines. The suitable choice of IHYPER depends on the formulation of the material model. For shells, there is also the special option of setting IHYPER = 3 which will make the deformation gradient computed from the nodal coordinates and in the global coordinate system. With this option the user must compute the stress in the local system of interest, whence a transformation matrix between the global and this local system is passed to the user material routines (qmat). The columns in this matrix correspond to local basis vectors expressed in global coordinates, and this is the system that stress needs to be computed in. The user must be aware that since the deformation gradient is calculated directly from the element deformation it may not be consistent with the theory of the element that is used for the material. To account for thickness changes due to membrane straining, there are routines subroutine usrshl_updatfs(f,t,s,e) real f(3,3),t(4),s(4),e that recompute the deformation gradient based on the thickness strain increment e, and the nodal thicknesses t. The current nodal thicknesses are stored in the history variables array immediately following the storage of the deformation gradient. This routine must be called with these four values as t. This subroutine is expected to produce a deformation f and the new thicknesses s. This routine is used to find the strain increment e giving zero thickness stress. Once zero thickness stress is obtained, the user needs to store the new thicknesses s in the history variables array, which is achieved by copying the new thicknesses s to the location for the nodal thicknesses. There is also a vectorized version of this routine called usrshl_updatfv. Sample code is provided in the object library. In the following, a Neo-Hookean material is used as an example of the usage of the deformation gradient in user-defined materials. With 𝜆 and 𝜇 being the Lame parameters in the linearized theory, the strain energy density for this material is given by APPENDIX A 𝜓 = 𝜆(ln(det𝐅))2 − 𝜇ln(det𝐅) + 𝜇(tr(𝐅𝑇𝐅) − 3) meaning that the Cauchy stress can be expressed as σ = det𝐅 (𝜆ln(det𝐅)𝐈 + 𝜇(𝐅𝐅𝑇 − 𝐈)). Sample user subroutine 45 subroutine umat45 (cm,eps,sig,epsp,hsv,dt1,capa, . etype,time,temp,failel,crv,nnpcrv,cma,qmat,elsiz,idele,reject) c c****************************************************************** c| Livermore Software Technology Corporation (LSTC) | c| ------------------------------------------------------------ | c| Copyright 1987-2008 Livermore Software Tech. Corp | c| All rights reserved | c****************************************************************** c c Neo-Hookean material (sample user subroutine) c c Variables c c cm(1)=first material constant, here young's modulus c cm(2)=second material constant, here poisson's ratio c . c . c . c cm(n)=nth material constant c c eps(1)=local x strain increment c eps(2)=local y strain increment c eps(3)=local z strain increment c eps(4)=local xy strain increment c eps(5)=local yz strain increment c eps(6)=local zx strain increment c c sig(1)=local x stress c sig(2)=local y stress c sig(3)=local z stress c sig(4)=local xy stress c sig(5)=local yz stress c sig(6)=local zx stress c c hsv(1)=1st history variable c hsv(2)=2nd history variable c . c . c . c . c hsv(n)=nth history variable c c dt1=current time step size c capa=reduction factor for transverse shear c etype: c eq."solid" for solid elements c eq."sld2d" for shell forms 13, 14, and 15 (2D solids) c eq."shl_t" for shell forms 25, 26, and 27 (shells with thickness c stretch) c eq."shell" for all other shell elements plus thick shell forms 1 c and 2 APPENDIX A c eq."tshel" for thick shell forms 3 and 5 c eq."hbeam" for beam element forms 1 and 11 c eq."tbeam" for beam element form 3 (truss) c eq."dbeam" for beam element form 6 (discrete) c eq."beam " for all other beam elements c c time=current problem time. c c temp=current temperature c c failel=flag for failure, set to .true. to fail an integration point, c if .true. on input the integration point has failed earlier c c crv=array representation of curves in keyword deck c c nnpcrv=# of discretization points per crv() c c cma=additional memory for material data defined by LMCA at c 6th field of 2nd crad of *DATA_USER_DEFINED c c elsiz=characteristic element size c c idele=element id c c reject (implicit only) = set to .true. if this implicit iterate is c to be rejected for some reason c c All transformations into the element local system are c performed prior to entering this subroutine. Transformations c back to the global system are performed after exiting this c routine. c c All history variables are initialized to zero in the input c phase. Initialization of history variables to nonzero values c may be done during the first call to this subroutine for each c element. c c Energy calculations for the dyna3d energy balance are done c outside this subroutine. c include 'nlqparm' include 'iounits.inc' include 'bk06.inc' character*5 etype dimension cm(*),eps(*),sig(*),hsv(*),crv(lq1,2,*),cma(*) logical failel c if (ncycle.eq.1) then call usermsg('mat45') endif c c compute lame parameters c xlambda=cm(1)*cm(2)/((1.+cm(2))*(1.-2.*cm(2))) xmu=.5*cm(1)/(1.+cm(2)) c if (etype.eq.'solid'.or.etype.eq.'shl_t'.or. 1 etype.eq.'sld2d'.or.etype.eq.'tshel') then c c deformation gradient stored in hsv(1),...,hsv(9) c c compute jacobian c detf=hsv(1)*(hsv(5)*hsv(9)-hsv(6)*hsv(8)) 1 -hsv(2)*(hsv(4)*hsv(9)-hsv(6)*hsv(7)) 2 +hsv(3)*(hsv(4)*hsv(8)-hsv(5)*hsv(7)) APPENDIX A c c compute left cauchy-green tensor c b1=hsv(1)*hsv(1)+hsv(4)*hsv(4)+hsv(7)*hsv(7) b2=hsv(2)*hsv(2)+hsv(5)*hsv(5)+hsv(8)*hsv(8) b3=hsv(3)*hsv(3)+hsv(6)*hsv(6)+hsv(9)*hsv(9) b4=hsv(1)*hsv(2)+hsv(4)*hsv(5)+hsv(7)*hsv(8) b5=hsv(2)*hsv(3)+hsv(5)*hsv(6)+hsv(8)*hsv(9) b6=hsv(1)*hsv(3)+hsv(4)*hsv(6)+hsv(7)*hsv(9) c c compute cauchy stress c detfinv=1./detf dmu=xmu-xlambda*log(detf) sig(1)=detfinv*(xmu*b1-dmu) sig(2)=detfinv*(xmu*b2-dmu) sig(3)=detfinv*(xmu*b3-dmu) sig(4)=detfinv*xmu*b4 sig(5)=detfinv*xmu*b5 sig(6)=detfinv*xmu*b6 c else if (etype.eq.'shell') then c c deformation gradient stored in hsv(1),...,hsv(9) c c compute part of left cauchy-green tensor c independent of thickness strain increment c b1=hsv(1)*hsv(1)+hsv(4)*hsv(4)+hsv(7)*hsv(7) b2=hsv(2)*hsv(2)+hsv(5)*hsv(5)+hsv(8)*hsv(8) b4=hsv(1)*hsv(2)+hsv(4)*hsv(5)+hsv(7)*hsv(8) c c secant iterations for zero normal stress c do iter=1,5 c c first thickness strain increment initial guess c assuming Poisson's ratio different from zero c if (iter.eq.1) then eps(3)=-xlambda*(eps(1)+eps(2))/(xlambda+2.*xmu) c c second thickness strain increment initial guess c else if (iter.eq.2) then sigold=sig(3) epsold=eps(3) eps(3)=0. c c secant update of thickness strain increment c else if (abs(sig(3)-sigold).gt.0.0) then deps=-(eps(3)-epsold)/(sig(3)-sigold)*sig(3) sigold=sig(3) epsold=eps(3) eps(3)=eps(3)+deps endif c c compute last row of deformation gradient c call compute_f3s(hsv(3),hsv(6),hsv(9),eps(3)) c c compute jacobian c detf=hsv(1)*(hsv(5)*hsv(9)-hsv(6)*hsv(8)) 1 -hsv(2)*(hsv(4)*hsv(9)-hsv(6)*hsv(7)) APPENDIX A 2 +hsv(3)*(hsv(4)*hsv(8)-hsv(5)*hsv(7)) c c compute normal component of left cauchy-green tensor c b3=hsv(3)*hsv(3)+hsv(6)*hsv(6)+hsv(9)*hsv(9) c c compute normal stress c detfinv=1./detf dmu=xmu-xlambda*log(detf) sig(1)=detfinv*(xmu*b1-dmu) sig(2)=detfinv*(xmu*b2-dmu) sig(3)=detfinv*(xmu*b3-dmu) sig(4)=detfinv*xmu*b4 c c exit if normal stress is sufficiently small c if (abs(sig(3)).le.1.e-5* 1 (abs(sig(1))+abs(sig(2))+abs(sig(4)))) goto 10 enddo c c compute remaining components of left cauchy-green tensor c 10 b5=hsv(2)*hsv(3)+hsv(5)*hsv(6)+hsv(8)*hsv(9) b6=hsv(1)*hsv(3)+hsv(4)*hsv(6)+hsv(7)*hsv(9) c c compute remaining stress components c sig(5)=detfinv*xmu*b5 sig(6)=detfinv*xmu*b6 c c material model only available for solids and shells c else cerdat(1)=etype call lsmsg(3,MSG_SOL+1151,ioall,ierdat,rerdat,cerdat,0) endif return end Implicit analysis For brick, and shell, thick shell and Hughes-Liu beam elements, a user-defined material model can also be run with implicit analysis. When an implicit analysis is requested in the input keyword deck, LS-DYNA calls the subroutine urtanh for bricks, urtans for shells and urtanb for beams with appropriate input data for the calculation of the material tangent modulus. For a scalar implementation, this routine in turn calls utanXX with all necessary input parameters including es(6,6) – material tangent modulus Again, XX is the number that matches MT on the material card. For a vectorized implementation, the routine utanXXv is called, this time with the corresponding vector block dsave(nlq,6,6) – material tangent modulus This subroutine builds the tangent modulus to be used for assembling the tangent stiffness matrix and must be provided by the user. This matrix is equal to the zero APPENDIX A matrix when entering the user-defined routine, it must be symmetric and if the local coordinate system option is invoked for bricks, then it should be expressed in this local system. For shell elements, it should be expressed in the co-rotational system defined for the current shell element. All transformations back to the global system are made after exiting the user-defined routine. A feature that can be made useful for improving convergence characteristics is the parameter reject, which can be set to .true. in the user material routine. The purpose of this parameter is to indicate something that renders the iteration unacceptable. An example of this something may be too much increase in plastic strain in one step, another is a criterion on the total strain increment. What LS-DYNA will do in this situation is to print a warning message ‘Material model rejected current iterate’ and retry the step with a smaller time step. If chosen carefully (by way of experimenting), this may result in a good trade-off between the number of implicit iterations per step and the step size for overall speed. If the material is hyper-elastic, there are push forward operations of tangent modulus tensor available in subroutine push_forward_4(dsave, f11,f21,f31,f12,f22,f32,f13,f23,f33,lft,llt) which performs a push forward operation on the tangent modulus tensor, and the corresponding scalar routine subroutine push_forward_4s(es, f11,f21,f31,f12,f22,f32,f13,f23,f33) In the latter subroutine all arguments are scalars whereas the corresponding entries in the vectorized routine are vectors of length nlq. The f11 to f33 are components of the deformation gradient. The following sample user subroutine illustrates how to implement the tangent stiffness modulus for the Neo-Hookean material above. The material tangent modulus is for this material given by 𝐂 = det𝐅 (𝜆𝐈 ⊗ 𝐈 + 2(𝜇 − 𝜆ln(det𝐅))𝐈). Sample user subroutine 42, tangent modulus subroutine utan42(cm,eps,sig,epsp,hsv,dt1,capa, . etype,tt,temper,es,crv) c****************************************************************** c| livermore software technology corporation (lstc) | c| ------------------------------------------------------------ | c| copyright 1987-1999 | c| all rights reserved | c****************************************************************** c c Neo-Hookean material tangent modulus (sample user subroutine) APPENDIX A cm(n)=nth material constant epsp=effective plastic strain c Variables c c cm(1)=first material constant, here young's modulus c cm(2)=second material constant, here poisson's ratio . c c . c . c c c eps(1)=local x strain increment c eps(2)=local y strain increment c eps(3)=local z strain increment c eps(4)=local xy strain increment c eps(5)=local yz strain increment c eps(6)=local zx strain increment c c sig(1)=local x stress c sig(2)=local y stress c sig(3)=local z stress c sig(4)=local xy stress c sig(5)=local yz stress c sig(6)=local zx stress c c c c hsv(1)=1st history variable c hsv(2)=2nd history variable c . c . c . c . c hsv(n)=nth history variable c c dt1=current time step size c capa=reduction factor for transverse shear c etype: c eq."brick" for solid elements c eq."shell" for all shell elements c eq."beam" for all beam elements c eq."dbeam" for all discrete beam elements c c tt=current problem time. c c temper=current temperature c c es=material tangent modulus c c c c c c c include 'nlqparm' character*(*) etype dimension cm(*),eps(*),sig(*),hsv(*),crv(lq1,2,*) dimension es(6,*) c c no history variables, NHV=0 c deformation gradient stored in hsv(1),...,hsv(9) c c compute jacobian c detf=hsv(1)*(hsv(5)*hsv(9)-hsv(6)*hsv(8)) 1 -hsv(2)*(hsv(4)*hsv(9)-hsv(6)*hsv(7)) 2 +hsv(3)*(hsv(4)*hsv(8)-hsv(5)*hsv(7)) crv=array representation of curves in keyword deck The material tangent modulus is set to 0 prior to entering this routine. It should be expressed in the local system upon exiting this routine. All transformations back to the global system is made outside this routine. APPENDIX A c c compute lame parameters c xlambda=cm(1)*cm(2)/((1.+cm(2))*(1.-2.*cm(2))) xmu=.5*cm(1)/(1.+cm(2)) c c compute tangent stiffness c same for both shells and bricks c detfinv=1./detf dmu=xmu-xlambda*log(detf) es(1,1)=detfinv*(xlambda+2.*dmu) es(2,2)=detfinv*(xlambda+2.*dmu) es(3,3)=detfinv*(xlambda+2.*dmu) es(4,4)=detfinv*dmu es(5,5)=detfinv*dmu es(6,6)=detfinv*dmu es(2,1)=detfinv*xlambda es(3,2)=detfinv*xlambda es(3,1)=detfinv*xlambda es(1,2)=es(2,1) es(2,3)=es(3,2) es(1,3)=es(3,1) c return end User-Defined Materials with Equations of State The following example umat44v is set up to be used with an equation of state (EOS). Unlike standard models, it updates only the deviatoric stress and it assigns a value to PC, the pressure cut-off. The pressure cut-off limits the amount of hydrostatic pressure that can be carried in tension (i.e., when the pressure is negative). The default value is zero, and a large negative number will allow the material to carry an unlimited pressure load in tension. It is calculated within the material model because it is typically a function of the current state of the material and varies with time. In this example, however, it is a constant value for simplicity. The pressure cut-off array is passed through the named common block eosdloc. Depending on the computing environment, compiler directives may be required (e.g., the task common directive in the example) for correct SMP execution. In addition, the number of history variables, NHV, must be increased by 4 in the input file to allocate the extra storage required for the EOS. The storage is the first 4 variables in hsvs, and it must not be altered by the user-defined material model. subroutine umat44v(cm,d1,d2,d3,d4,d5,d6,sig1,sig2, . sig3,sig4,sig5,sig6,eps,hsvs,lft,llt,dt1siz,capa, . etype,tt,temps,failels,nlqa,crv) parameter (third=1.0/3.0) include 'nlqparm' c c*** isotropic plasticity with linear hardening c c*** updates only the deviatoric stress so that it can be used with c an equation of state c character*5 etype APPENDIX A logical failels c C_TASKCOMMON (eosdloc) common/eosdloc/pc(nlq) c dimension cm(*),d1(*),d2(*),d3(*),d4(*),d5(*),d6(*), & sig1(*),sig2(*),sig3(*),sig4(*),sig5(*),sig6(*), & eps(*),hsvs(nlqa,*),dt1siz(*),temps(*),crv(lq1,2,*), & failels(*) c c*** shear modulus, initial yield stress, hardening, and pressure cut-off g =cm(1) sy0 =cm(2) h =cm(3) pcut=cm(4) c ofac=1.0/(3.0*g+h) twog=2.0*g c do i=lft,llt c c*** trial elastic deviatoric stress davg=third*(d1(i)+d2(i)+d3(i)) savg=third*(sig1(i)+sig2(i)+sig3(i)) sig1(i)=sig1(i)-savg+twog*(d1(i)-davg) sig2(i)=sig2(i)-savg+twog*(d2(i)-davg) sig3(i)=sig3(i)-savg+twog*(d3(i)-davg) sig4(i)=sig4(i)+g*d4(i) sig5(i)=sig5(i)+g*d5(i) sig6(i)=sig6(i)+g*d6(i) c c*** radial return aj2=sqrt(1.5*(sig1(i)**2+sig2(i)**2+sig3(i)**2)+ & 3.0*(sig4(i)**2+sig5(i)**2+sig6(i)**2)) sy=sy0+h*eps(i) eps(i)=eps(i)+ofac*max(0.0,aj2-sy) synew=sy0+h*eps(i) scale=synew/max(synew,aj2) c c*** scaling for radial return. note that the stress is now deviatoric. sig1(i)=scale*sig1(i) sig2(i)=scale*sig2(i) sig3(i)=scale*sig3(i) sig4(i)=scale*sig4(i) sig5(i)=scale*sig5(i) sig6(i)=scale*sig6(i) c c*** set pressure cut-off pc(i)=pcut c enddo c return end Post-processing a user-defined material Post-processing a user-defined material is very similar to post-processing a regular LS- DYNA material. There are however some things that are worth being stressed, all dealing with how to post-process history variables. APPENDIX A First, the effective plastic strain is always written to the d3plot database and thus need not be requested by the user. It is in LS-PRE/POST treated just as it is for any other LS- DYNA material. The number of additional history variables written to the d3plot database must be requested as the parameter NEIPH (for bricks) or NEIPS (for shells) on *DATABASE_ EXTENT_BINARY. For instance, if NEIPH (NEIPS) equals 2 the first two history variables in the history variables array are obtained as history var#1 and history var#2 in the d3plot database. By putting NEIPH (NEIPS) equal to NHV, all history variables are written to the d3plot database. Furthermore, if the material uses the deformation gradient (IHYPER = 1) an additional 9 variables must be requested to make this available for post-processing, i.e., put NEIPH (NEIPS) equal to NHV+9. This makes the deformation gradient available in the d3plot database as history variables NHV+1 to NHV+9, note however that for shells it is expressed in the co-rotational system. If the local coordinate system option (IORTHO = 1) is used, then the deformation gradient is expressed in this local system. To make the deformation gradient in the global system for bricks and co-rotational system for shells available and stored as history variables NHV+10 to NHV+18, NEIPH (NEIPS) is put equal to NHV+9+9(=NHV+18). APPENDIX B APPENDIX B: User Defined Equation of State The user can supply his/her own subroutines defining equation of state (EOS) models in LS-DYNA. To invoke a user-defined EOS, one must 1. Write a user EOS subroutine that is called by the LS-DYNA user EOS interface. 2. Create a custom executable which includes the EOS subroutine. 3. Invoke that subroutine by defining a part in the keyword input deck that uses *EOS_USER_DEFINED with the appropriate input parameters. Subroutine ueoslib and sample subroutines ueos21s and ueos21v are provided in the file dyn21b.f. This text serves as an introductory guide to implementing such a model. Note that names of variables and subroutines below may differ from the actual ones depending on platform and current version of LS-DYNA. General overview When the keyword *EOS_USER_DEFINED is defined for a part in the keyword deck, LS- DYNA calls the subroutine ueoslib with the appropriate input data for the EOS update. This subroutine is called twice for each integration point in each element. The first call requires the EOS to calculate the bulk modulus, and the second updates the pressure and internal energy. In these routines, which may be modified by the user if necessary, the following data structures are initialized for the purpose of being supplied to a specific scalar material subroutine. iflag – mode flag EQ.-1: for initializing EOS constants EQ.0: for calculating the bulk modulus EQ.1: for the pressure and energy update cb – bulk modulus pnew – the new pressure rho0 – reference density hist – array of user-defined history variables NHV in length specen – internal energy per unit reference volume df – volume ratio, V/V0 v0 – the initial volume. dvol – volume increment pc – pressure cut-off APPENDIX B If the vectorization flag is active (IVECT = 1) on the EOS card, variables are, in general, stored in vector blocks of length nlq, with vector indices ranging from lft to llt , which allows for a more efficient execution of the EOS routine. As an example, the data structures mentioned above for the vectorized case are cb(nlq) – bulk modulus pnew(nlq) – the new pressure hist(nlq,*) – array of user-defined history variables with NHV columns specen(nlq) – internal energy per unit reference volume df(nlq) – volume ratio, V/V0 v0(nlq) – the initial volume dvol(nlq) – volume increment pc(nlq) – pressure cut-off The value of nlq is set as a parameter in the include file nlqparm, included at the top of the subroutine, and varies between machines and operating systems. Each entry in a vector block is associated with an element in the finite element mesh for a fix integration point. The number of entries in the history variables array (indicated by * in the above) matches the number of history variables requested on the material card (NHV). All history variables are initially zero and are initialized within the EOS on the first time step, when the logical variable first, passed through the argument list, is .TRUE. Furthermore, all user-defined EOS models require a bulk modulus, cb, for transmitting boundaries, contact interfaces, rigid body constraints, and time step calculations. In addition to the variables mentioned above, the following data can be supplied to the user material routines, regardless of whether vectorization is used or not. eosp(*) – array of material constants from the input file tt – current time crv(lq1,2,*) – array representation of curves defined in the keyword deck. A user defined EOS subroutine, ueosXXs in the scalar case or ueosXXv in the vector case, will be called for parts that point to *EOS_USER_DEFINED in the input deck. The letters XX stand for a number between 21 and 30 that matches the input variable EOST in the *EOS_USER_DEFINED keyword. During the initialization phase, the EOS is called with iflag = -1 to permit the initialization of constants in the user EOS. Although fewer than 48 constants may be read into the array eosp during the input, the user may use all 48 within the EOS subroutines. The user defined subroutine should calculate the bulk modulus when iflag = 0, and update the pressure, internal energy and history variables when iflag = 1. The use of curves (*DEFINE_CURVE) is discussed in Appendix A. A sample scalar user subroutine for a Gruneisen EOS is provided below and it is immediately followed by its vector counterpart. APPENDIX B Sample user subroutine 21 subroutine ueos21s(iflag,cb,pnew,hist,rho0,eosp,specen, & df,dvol,v0,pc,dt,tt,crv,nnpcrv,first) include 'nlqparm' c c*** example scalar user implementation of the Gruneisen EOS c c*** variables c iflag ----- =0 calculate bulk modulus c =1 update pressure and energy c cb -------- bulk modulus c pnew ------ new pressure c hist ------ history variables c rho0 ------ reference density c eosp ------ EOS constants c specen ---- energy/reference volume c df -------- volume ratio, v/v0 = rho0/rho c dvol ------ change in volume over time step c v0 -------- reference volume c pc -------- pressure cut-off c dt -------- time step size c tt -------- current time c crv ------- curve array c nnpcrv ---- number of points in each curve c first ----- logical .true. for tt,crv,first time step c (for initialization of the history variables) c logical first c dimension hist(*),eosp(*),crv(lq1,2,*) integer nnpcrv(*) c c =eosp(1) s1 =eosp(2) s2 =eosp(3) s3 =eosp(4) g0 =eosp(5) sa =eosp(6) s11=s1-1. s22=2.*s2 s33=3.*s3 s32=2.*s3 sad2=.5*sa g0d2=1.-.5*g0 roc2=rho0*c**2 c c*** calculate the bulk modulus for the EOS contribution to the sound speed if (iflag.eq.0) then xmu=1.0/df-1. dfmu=df*xmu facp=.5*(1.+sign(1.,xmu)) facn=1.-facp xnum=1.+xmu*(+g0d2-sad2*xmu) xdem=1.-xmu*(s11+dfmu*(s2+s3*dfmu)) tmp=facp/(xdem*xdem) a=roc2*xmu*(facn+tmp*xnum) b=g0+sa*xmu pnum=roc2*(facn+facp*(xnum+xmu*(g0d2-sa*xmu))) pden=2.*xdem*(-s11 +dfmu*(-s22+dfmu*(s2-s33+s32*dfmu))) cb=pnum*(facn+tmp)-tmp*a*pden+sa*specen+ & b*df**2*max(pc,(a+b*specen)) c c*** update the pressure and internal energy else xmu=1.0/df-1. APPENDIX B dfmu=df*xmu facp=.5*(1.+sign(1.,xmu)) facn=1.-facp xnum=1.+xmu*(+g0d2-sad2*xmu) xdem=1.-xmu*(s11+dfmu*(s2+s3*dfmu)) tmp=facp/(xdem*xdem) a=roc2*xmu*(facn+tmp*xnum) b=g0+sa*xmu dvov0=0.5*dvol/v0 denom=1.+ b*dvov0 pnew=(a+specen*b)/max(1.e-6,denom) pnew=max(pnew,pc) specen=specen-pnew*dvov0 endif c return end subroutine ueos21v(lft,llt,iflag,cb,pnew,hist,rho0,eosp,specen, & df,dvol,v0,pc,dt,tt,crv,nnpcrv,first) include 'nlqparm' c c*** example vectorized user implementation of the Gruneisen EOS c c*** variables c lft,llt --- tt,crv,first and last indices into arrays c iflag ----- =0 calculate bulk modulus c =1 update pressure and energy c cb -------- bulk modulus c pnew ------ new pressure c hist ------ history variables c rho0 ------ reference density c eosp ------ EOS constants c specen ---- energy/reference volume c df -------- volume ratio, v/v0 = rho0/rho c dvol ------ change in volume over time step c v0 -------- reference volume c pc -------- pressure cut-off c dt -------- time step size c tt -------- current time c crv ------- curve array c nnpcrv ---- number of points in each curve c first ----- logical .true. for tt,crv,first time step c (for initialization of the history variables) c logical first c dimension cb(*),pnew(*),hist(nlq,*),eosp(*), & specen(*),df(*),dvol(*),pc(*),v0(*) dimension crv(lq1,2,*) integer nnpcrv(*) c c =eosp(1) s1 =eosp(2) s2 =eosp(3) s3 =eosp(4) g0 =eosp(5) sa =eosp(6) s11=s1-1. s22=2.*s2 s33=3.*s3 s32=2.*s3 sad2=.5*sa g0d2=1.-.5*g0 roc2=rho0*c**2 c c*** calculate the bulk modulus for the EOS contribution to the sound speed APPENDIX B if (iflag.eq.0) then do i=lft,llt xmu=1.0/df(i)-1. dfmu=df(i)*xmu facp=.5*(1.+sign(1.,xmu)) facn=1.-facp xnum=1.+xmu*(+g0d2-sad2*xmu) xdem=1.-xmu*(s11+dfmu*(s2+s3*dfmu)) tmp=facp/(xdem*xdem) a=roc2*xmu*(facn+tmp*xnum) b=g0+sa*xmu pnum=roc2*(facn+facp*(xnum+xmu*(g0d2-sa*xmu))) pden=2.*xdem*(-s11 +dfmu*(-s22+dfmu*(s2-s33+s32*dfmu))) cb(i)=pnum*(facn+tmp)-tmp*a*pden+sa*specen(i)+ & b*df(i)**2*max(pc(i),(a+b*specen(i))) enddo c c*** update the pressure and internal energy else do i=lft,llt xmu=1.0/df(i)-1. dfmu=df(i)*xmu facp=.5*(1.+sign(1.,xmu)) facn=1.-facp xnum=1.+xmu*(+g0d2-sad2*xmu) xdem=1.-xmu*(s11+dfmu*(s2+s3*dfmu)) tmp=facp/(xdem*xdem) a=roc2*xmu*(facn+tmp*xnum) b=g0+sa*xmu dvov0=0.5*dvol(i)/v0(i) denom=1.+b*dvov0 pnew(i)=(a+specen(i)*b)/max(1.e-6,denom) pnew(i)=max(pnew(i),pc(i)) specen(i)=specen(i)-pnew(i)*dvov0 enddo endif c return end The Gruneisen EOS implemented in the example subroutines has the same form as *EOS_GRUNEISEN, EOS Form 4. Its update of the pressure and the internal energy are typical for an EOS that is linear in the internal energy, 𝑃 = 𝐴(𝜌) + 𝐵(𝜌)𝐸 where A and B correspond to the variables a and b in the example subroutines, and E is specen. Integrating the energy equation with the trapezoidal rule gives 𝐸𝑛+1 = 𝐸𝑛 + (𝜎 ′𝑛 + 𝜎 ′𝑛+1 )Δ𝜀 − (𝑃𝑛 + 𝑞𝑛 + 𝑃𝑛+1 + 𝑞𝑛+1 ) Δ𝑉 𝑉0 where the superscripts refer to the time step, Δ𝑉 is the change in the volume associated with the Gauss point and V0 is the reference volume. Collecting all the energy contributions on the right hand side except for the contribution from the new pressure gives a simple linear relationship between the new internal energy and pressure, 𝐸𝑛+1 = 𝐸̃ − 𝑃𝑛+1Δ𝑉 2𝑉0 . APPENDIX B The value of specen passed to ueosXX for the pressure and energy update corresponds to𝐸̃. Substituting this relation into the EOS and solving for the new pressure gives 𝑃𝑛+1 = 𝐴𝜌𝑛+1 + 𝐵𝜌𝑛+1𝐸̃ 1 + 𝐵Δ𝑉 2𝑉0 . The final update of the new energy is calculated using the new pressure. For a more general EOS, the nonlinear equation in the new pressure, 𝑃𝑛+1 = 𝑃 (𝜌𝑛+1, 𝐸̃ − 𝑃𝑛+1Δ𝑉 2𝑉0 ) is solved iteratively using Newton iteration or successive substitution. The pressure cut-off, pc, is used to limited the amount of pressure that can be generated by tensile loading, pnew=max(pnew,pc). Its value is usually specified in the *MAT input, e.g., *MAT_JOHNSON_COOK. It is not enforced outside of the EOS subroutines, and it is up to the user to determine whether or not to enforce the pressure cut-off in ueosXX. If the user does enforce it, the pressure cut-off should be applied before the final update to the internal energy otherwise the energy will be incorrect. Many of the calculations performed to calculate the bulk modulus are the same as those for updating the pressure and energy. Since the bulk modulus calculation always precedes the pressure update, the values may be saved in a common block during the bulk modulus calculation to reduce the cost of the pressure update. The arrays used to store the values in the vectorized subroutines should be dimensioned by nlq. One of the most common errors in implementing an EOS from a paper or book is the use of the wrong internal energy. There are three internal energies in common use: the energy per unit mass,𝑒𝑀, the energy per unit current volume,𝑒𝑉, and the energy per unit reference volume, E. LS-DYNA always uses the energy per unit reference volume. Some useful relations for converting between EOS in the literature and the variables in LS-DYNA are 𝑒𝑉 = 𝐸 𝑒𝑀 = 𝐸 = = 𝑉0 𝑉0 𝑉0 specen df specen rho0 rho0 df 𝜌 = 𝜌0 = APPENDIX C APPENDIX C: User Defined Element Interface for Solids and Shells In this appendix the user-defined element interface for solids and shells is described. The interface can accommodate either an integrated or a resultant element. For the integrated element, the user needs to supply two matrices defining the kinematical properties of the element, and choose between using standard LS-DYNA hourglass stabilization, a user-defined stabilization, or no stabilization when zero energy modes are not present. The number and location of the integration points is arbitrary, i.e., user-defined. For the resultant/discrete element formulations, the force and stiffness assembly must also be implemented. History variables can be associated with the user defined elements. If desired, the element may utilize more than the conventional 3 (for bricks) and 6 (for shells) degrees-of-freedom per node. The user element is implemented according to how standard elements are implemented in LS-DYNA with the exception that two user routines are called for setting up the matrices of interest. In the end, the gradient-displacement matrix 𝐵𝑖𝑗𝑘𝐾 is constructed with the property that 𝐵𝑖𝑗𝑘𝐾𝑢𝑘𝐾 = ∂𝑣𝑖 ∂𝑥𝑗 where 𝑢𝑘𝐾 is the vector of velocity nodal degrees of freedom and the right hand side is the velocity gradient. Moreover, the determinant 𝐽 of the jacobian matrix determining the mapping from the isoparametric to physical domain is needed for numerical integration. From these expressions, the strains are determined as the symmetric part of the velocity gradient and the spin as the corresponding antisymmetric part. The stresses are evaluated using the constitutive models in LS-DYNA and the internal forces are obtained from 𝑓𝑘𝐾 = ∫ 𝜎𝑖𝑗𝐵𝑖𝑗𝑘𝐾𝑑𝑉 where 𝜎𝑖𝑗 are the stresses. Furthermore, the geometric and material tangent stiffnesses are obtained through and 𝐾𝑖𝐼𝑗𝐽 mat = ∫ 𝐶𝑘𝑙𝑚𝑛𝐵𝑘𝑙𝑖𝐼𝐵𝑚𝑛𝑗𝐽𝑑𝑉 geo = ∫ 𝜎𝑚𝑛𝐵𝑘𝑚𝑖𝐼𝐵𝑘𝑛𝑗𝐽𝑑𝑉 𝐾𝑖𝐼𝑗𝐽 where 𝐶𝑘𝑙𝑚𝑛 is the tangent modulus for the material. The integrals are evaluated using user-defined quadrature using the determinant 𝐽. APPENDIX C For user-defined hourglass control, the user must provide the corresponding internal force and stiffness contribution in a separate user routine. There is also the option to provide the force and stiffness matrix directly for the entire element. To invoke a user-defined element one must do the following: 1. Write user element subroutine that defines the kinematics or kinetics of the element. 2. Create a custom executable which includes these subroutines. 3. Invoke the element by specifying this on the corresponding *SECTION card. The dummy subroutines for the user defined elements are provided to the user in a FORTRAN source file for you to modify along with the necessary object files to compile a new executable. Contact LSTC or your local distributor for information about how to obtain these files as well as what compiler/version to use for your specific platform. Up to five user elements can simultaneously be used for bricks and shells (i.e. a total of ten). This text serves as an introductory guide on how to implement such an element. General overview To activate a user-defined element, it is necessary to set ELFORM to a number between 101 and 105 on the *SECTION definition. By doing so, the kinematics of the elements in the corresponding part will be determined from calling the subroutine subroutine uXXX_bYYY(bmtrx,gmtrx,gjac,... ⋮ dimension bmtrx(nlq,3,3,*),gmtrx(nlq,3,3),gjac(*) where XXX is substituted for shl for a shell-section and sld for a solid-section and YYY is the number specified in position ELFORM. Depending on the choice of ITAJ in the input, the user should set the matrices as follows. If ITAJ = 0, then set the isoparametric gradient-displacement matrix, represented by the array bmtrx , and jacobian matrix, represented by the array gmtrx. Here, the first index corresponds to the LS-DYNA block loop index where nlq is the block size. For a more convenient notation in the following, we assign a correspondence between the arrays gmtrx and bmtrx in the subroutines to matrices/tensors as follows gmtrx(*,i,j) - 𝑔𝑖𝑗 bmtrx(*,i,j,k) - 𝑏𝑖𝑗𝑘 These matrices should be determined so that at the current integration point: APPENDIX C 𝑔𝑖𝑗 = 𝑏𝑖𝑗𝑘𝑢𝑘 = ∂𝑥𝑖 ∂𝜉𝑗 ∂𝑣𝑖 ∂𝜉𝑗 Δ𝑡 In the above, summation over repeated indices is assumed. We use the following notation: 𝑥𝑖(𝜉1, 𝜉2, 𝜉3, 𝑡) = ith component of the current position vector at the isoparametric coordinate (𝜉1, 𝜉2, 𝜉3) and time t. 𝑣𝑖(𝜉1, 𝜉2, 𝜉3, 𝑡) = ith component of the velocity vector at the isoparemetric coordinate (𝜉1, 𝜉2, 𝜉3) and time t. Δ𝑡 = current time step 𝑢𝑘 = kth component of generalized local displacements 𝜉𝑖 = ith component of the isoparametric coordinate ranging from - 1.0 to 1.0 For shells, there is an option to get all variables in either the LS-DYNA local coordinate system (ILOC=0) or in the global coordinate system (ILOC=1). The matrix for the coordinate system transformation is also passed to the user routines where the columns represent the local unit base vectors. The resulting strains must always be in the local coordinate system for the constitutive evaluations. For no extra degrees of freedom , the index 𝑘 in the displacement expression is determined from the formula 𝑘 = 𝑛(𝑚 − 1) + 𝑑 where 𝑛 = 3 if only translational degrees of freedom are present (typical for solids) and 𝑛 = 6 if rotational degrees of freedom are present (typical for shells), 𝑚 is the local node number (𝑚 = 1,2, . ..) and 𝑑 is the degree of freedom. The translational degrees of freedom correspond to 𝑑 ≤ 3 and the rotational degrees of freedom to 4 ≤ 𝑑 ≤ 6. If ITAJ=1, the user should set up the physical gradient-displacement matrix, represented by the array bmtrx, and jacobian determinant, represented by the array gjac. Again, we assign a correspondence between the arrays gjac and bmtrx in the subroutines to matrices/tensors as follows gjac(*) - 𝐽 bmtrx(*,i,j,k) - 𝑏𝑖𝑗𝑘 These matrices should be determined so that at the current integration point: 𝐽 = det ∂𝑥𝑖 ∂𝜉𝑗 APPENDIX C 𝑏𝑖𝑗𝑘𝑢𝑘 = ∂𝑣𝑖 ∂𝑥𝑗 Δ𝑡 To be able to set up these matrices, a set of additional auxiliary variables are passed to the user element subroutines. These include the isoparametric coordinate, the element thickness, and the shape function values, and derivatives. Again, for shells these are expressed in either the local or global coordinate system depending on the user’s choice. For more information on these variables, the user is referred to the comments in the subroutines. The integrated elements can use up to a total of 100 integration points (in the plane for shells) at arbitrary locations. These must be specified in terms of isoparametric coordinates and weights following the first of the user-defined cards in the *SECTION_ … input. The isoparametric coordinates should range from –1 to 1 and the weights should sum up to 4 for shells and 8 for solids. It may be necessary to incorporate hourglass stabilization to suppress zero energy modes, this is done by putting IHGF.GT.0 in the input. For IHGF.EQ.1, the LS- DYNA hourglass routines are used automatically and for IHGF.EQ.2 or IHGF.EQ.3 the user must provide hourglass force and stiffness in a specific user-defined routine. If IHGF.EQ.3, physical stabilization becomes available since the resultant material tangent moduli are passed to the hourglass routine to provide the current membrane, bending and coupled membrane-bending stiffness of the material. With 𝐶𝑖𝑗 denoting the material tangent modulus in matrix form, the resultant tangent moduli are expressed as (membrane) 𝐶̅ 0 = ∫ 𝐶𝑖𝑗 𝑑𝑉 𝑖𝑗 𝐶̅ 1 = ∫ 𝑧1𝐶𝑖𝑗 𝑑𝑉 (membrane − bending) 𝑖𝑗 𝐶̅ 2 = ∫ 𝑧2𝐶𝑖𝑗 𝑑𝑉 (bending) 𝑖𝑗 where 𝑧 is the thickness coordinate for shells. For solids, only the first resultant modulus is passed. In this case the array has 21 entries that correspond to the subdiagonal terms of the 6 by 6 resultant matrix. For the matrix index (𝑖, 𝑗) in the material tangent modulus matrix, where 𝑖 ≥ 𝑗, the index 𝐼 of the array passed to the routine is given by 𝐼 = 𝑖(𝑖 − 1)/2 + 𝑗 i.e., the subdiagonal terms are stored row-wise in the array. For shells, all three moduli are passed in the local coordinate system where each array has 15 entries corresponding to the subdiagonal terms of the 5 by 5 resultant matrices. The through thickness direction is here eliminated from the plane stress assumption. The formula for the array indices transformation above holds. This subroutine is called subroutine uXXX_eYYY(force,stiff,ndtot,... ⋮ APPENDIX C dimension force(nlq,*),stiff(nlq,ndtot,*) where again XXX and YYY should be substituted as described for the other subroutines in the above. The variables in the subroutine corresponds to the force and stiffness as force(*,i) - 𝑓𝑖 stiff(*,i,j) - 𝐾𝑖𝑗 where the indices corresponds to node and degree of freedom numbers exactly as for the displacements. For shells the force and stiffness is set up in the local element system (ILOC=0) or global system (ILOC=1). The variable ndtot is the total number of degrees of freedom for the element. Passed to this subroutine are also the property parameters and history variables associated with the element. The values of the property parameters are defined in the input of a user-defined element. No more than 40 property parameters and 100 history variables can be used for each user-defined element. The history variables must be updated in this routine by the user. Resultant/discrete elements By putting NIP(P) equal to 0 in the input, a resultant/discrete element is assumed. For this option (which is incompatible with IHGF.GT.0) the user must provide force and stiffness in the same user-defined routine as for the user-defined hourglass control. This means that no material routine is called to update stresses and history variables, rather stresses and history variables are to be updated from within the user element routine. Nevertheless, the user should define *MAT_ELASTIC as the material for the corresponding part with suitable values of the Young’s modulus and Poisson’s ratio. These material properties are used to calculate the time step and for determining contact stiffnesses. Again, property parameters and history variables are passed to the routine, and for shells also the thicknesses of the elements. For the shell thickness update option (ISTUPD.GT.0 on *CONTROL_SHELL) it is up to the user to update the thicknesses in this routine. For this option, and this option only, the stiffness matrix assembled in the element routines can be input as nonsymmetric if LCPACK=3 on *CONTROL_IMPLICIT_SOLVER, i.e., if the nonsymmetric solver is used to update the Newton iterates. In what follows, a short description of the additional features associated with the user elements is given. Nodal fiber vectors If a user-defined shell element formulation uses the nodal fiber vectors, this must be specified by putting IUNF=1 on the *SECTION_SHELL card. With this option the nodal APPENDIX C fiber vectors are processed in the element routines and can be used as input for determining the 𝑏𝑖𝑗𝑘, 𝑔𝑖𝑗/𝐽, 𝑓𝑖 and 𝐾𝑖𝑗 tensors/matrices in the user routines. If not, it is assumed that the fiber direction is normal to the plane of the shell at all times. These are expressed in either the local or global system depending on the user’s choice. See comments in the subroutines for more information. Extra degrees of freedom Exotic element formulations may require extra degrees-of-freedom per node besides the translational (and rotational) degrees-of-freedom. Currently, up to 3 extra degrees of freedom per node can be used for user-defined elements. To use extra degrees of freedom, a scalar node must be defined for each node that makes up the connectivity of the user element. A scalar node is defined using the keyword *NODE_SCALAR_VALUE, in which the user also prescribe initial and boundary conditions associated with the extra variables. The connectivity of the user elements must then be specified with the option *ELEMENT_SOLID_DOF or *ELEMENT_SHELL_DOF, where an extra line is used to connect the scalar nodes to the element. As an example: *NODE_SCALAR_VALUE $ NID V1 V2 V3 NDF 11 1.0 1 12 1.0 1 13 1.0 1 14 1.0 1 *ELEMENT_SHELL_DOF $ EID PID N1 N2 N3 N4 1 1 1 2 3 4 $ NS1 NS2 NS3 NS4 11 12 13 14 defines an element with one extra degree of freedom. The initial value of the corresponding variable is 1.0 and it is unconstrained. Finally, the user sets the parameter NXDOF on the *SECTION_… card to 1, 2 or 3 depending on how many extra degrees of freedom that should be used in the user-defined element. An array xdof containing the current values of these extra variables are passed to the user routines for setting up the correct kinematical properties, see comments in the routines for more information. The formula for the displacement index changes to 𝑘 = (𝑛 + 𝑛𝑥𝑑𝑜𝑓 )(𝑚 − 1) + 𝑑 where 𝑛𝑥𝑑𝑜𝑓 is the number of extra degrees of freedom. The extra degrees of freedom for each node corresponds to 𝑛 + 1 ≤ 𝑑 ≤ 𝑛 + 𝑛𝑥𝑑𝑜𝑓 . For dynamic simulations, the mass corresponding to these extra nodes are defined using *ELEMENT_INERTIA or *ELEMENT_MASS. APPENDIX C Related keywords: The following is a list of keywords that apply to the user defined elements The *SECTION_SHELL card A third card with accompanying optional cards of the *SECTION_SHELL keyword must be added if the user defined element option is invoked Additional Card for ELFORM = 101,102,103,104 or 105 Card 3 1 2 3 4 5 6 7 8 Variable NIPP NXDOF IUNF IHGF ITAJ LMC NHSV ILOC Type Default I 0 I 0 I 0 I 0 I 0 I 0 I 0 I 0 Include NIPP cards according to the following format. Card 4 Variable Type 1 XI F 2 3 4 5 6 7 8 ETA WGT F F Define LMC property parameters using 8 parameters per card. Card 5 Variable 1 P1 Type F 2 P2 F 3 P3 F 4 P4 F 5 P5 F 6 P6 F 7 P7 F 8 P8 F VARIABLE ELFORM DESCRIPTION GT.100.AND.LT.106: User-defined shell NIPP Number of in-plane integration points for user-defined shell (0 if resultant element) APPENDIX C VARIABLE NXDOF DESCRIPTION Number of extra degrees of freedom per node for user-defined shell IUNF Flag for using nodal fiber vectors in user-defined shell EQ.0: Nodal fiber vectors are not used . EQ.1: Nodal fiber vectors are used IHGF Flag for using hourglass stabilization (NIPP.GT.0) EQ.0: Hourglass stabilization is not used EQ.1: LS-DYNA hourglass stabilization is used EQ.2: User-defined hourglass stabilization is used EQ.3: Same as 2, but the resultant material tangent moduli are passed ITAJ Flag for setting up finite element matrices (NIPP.GT.0) EQ.0: Set up matrices wrt isoparametric domain EQ.1: Set up matrices wrt physical domain LMC Number of property parameters NHSV Number of history variables ILOC Local coordinate system option EQ.0: All variables are passed in the local element system EQ.1: All variables are passed in the global system XI ETA WGT PI First isoparametric coordinate Second isoparametric coordinate Isoparametric weight Ith property parameter For more information on the variables the user may consult the previous sections in this appendix. APPENDIX C The *SECTION_SOLID card A second card with accompanying optional cards of the *SECTION_SOLID keyword must be added if the user defined elements option is invoked. Additional card for ELFORM = 101,102,103,104 or 105 Card 3 1 2 3 4 5 6 7 8 Variable NIP NXDOF IHGF ITAJ LMC NHSV Type Default I 0 I 0 I 0 I 0 I 0 I 0 Include NIP cards according to the following format. Card 4 Variable Type 1 XI F 2 3 4 5 6 7 8 ETA ZETA WGT F F F Define LMC property parameters using 8 parameters per card. Card 5 Variable 1 P1 Type F 2 P2 F 3 P3 F 4 P4 F 5 P5 F 6 P6 F 7 P7 F 8 P8 F VARIABLE ELFORM NIP NXDOF DESCRIPTION GT.100.AND.LT.106: User-defined solid Number of integration points for user-defined solid (0 if resultant element) Number of extra degrees of freedom per node for user-defined solid APPENDIX C VARIABLE DESCRIPTION IHGF Flag for using hourglass stabilization (NIP.GT.0) EQ.0: Hourglass stabilization is not used EQ.1: LS-DYNA hourglass stabilization is used EQ.2: User-defined hourglass stabilization is used EQ.3: Same as 2, but the resultant material tangent moduli are passed ITAJ Flag for setting up finite element matrices (NIP.GT.0) EQ.0: Set up matrices wrt isoparametric domain EQ.1: Set up matrices wrt physical domain LMC Number of property parameters NHSV Number of history variables XI ETA ZETA WGT First isoparametric coordinate Second isoparametric coordinate Third isoparametric coordinate Isoparametric weight PI Ith property parameter For more information on the variables the user may consult the previous sections in this appendix. Sample User Shell Element 101 (Belytschko-Tsay shell) The geometry of the Belytschko-Tsay element in local coordinates can be written 𝑥𝑖 = (𝑥𝑖𝐼 + 𝑣𝑖 = (𝑣𝑖𝐼 + 𝜉3𝛿𝑖3)𝑁𝐼(𝜉1, 𝜉2) 𝜉3𝑒𝑖𝑗3𝜔𝑗𝐼)𝑁𝐼(𝜉1, 𝜉2) Where, 𝑥𝑖𝐼 = 𝑖th component of coordinate of node𝐼 𝑣𝑖𝐼 = 𝑖th component of translational velocity of node 𝐼 𝜔𝑗𝐼 = 𝑗th component of rotational velocity of node 𝐼 APPENDIX C 𝑡 = thickness of element 𝑒𝑖𝑗𝑘 = permutation tensor 𝑁𝐼 = shape function localized at node 𝐼 𝛿𝑖3 = Kronecker delta Taking the derivative of these expressions with respect to the isoparametric coordinate yields and 𝜉3𝛿𝑖3) 𝜉3𝛿𝑖3) ∂𝑁𝐼 ∂𝜉1 ∂𝑁𝐼 ∂𝜉2 ∂𝑥𝑖 ∂𝜉1 ∂𝑥𝑖 ∂𝜉2 ∂𝑥𝑖 ∂𝜉3 = (𝑥𝑖𝐼 + = (𝑥𝑖𝐼 + = 𝛿𝑖3 ∂𝑣𝑖 ∂𝜉1 ∂𝑣𝑖 ∂𝜉2 ∂𝑣𝑖 ∂𝜉3 = (𝑣𝑖𝐼 + = (𝑣𝑖𝐼 + 𝜉3𝑒𝑖𝑗3𝜔𝑗𝐼) 𝜉3𝑒𝑖𝑗3𝜔𝑗𝐼) ∂𝑁𝐼 ∂𝜉1 ∂𝑁𝐼 ∂𝜉2 = 𝑒𝑖𝑗3𝜔𝑗𝐼𝑁𝐼 respectively. Using these expressions the element is implemented as a user-defined shell as follows. subroutine ushl_b101(bmtrx,gmtrx,gjac, 1 xi,eta,zeta, 2 n1,n2,n3,n4, 3 dn1dxi,dn2dxi,dn3dxi,dn4dxi, 4 dn1deta,dn2deta,dn3deta,dn4deta, 5 x1,x2,x3,x4,y1,y2,y3,y4,z1,z2,z3,z4, 6 xdof, 7 thick,thck1,thck2,thck3,thck4, 8 fx1,fx2,fx3,fx4, 9 fy1,fy2,fy3,fy4, . fz1,fz2,fz3,fz4, . gl11,gl21,gl31,gl12,gl22,gl32,gl13,gl23,gl33, . lft,llt) include 'nlqparm' c c Compute b and g matrix for user-defined shell 101 c dimension bmtrx(nlq,3,3,*),gmtrx(nlq,3,3),gjac(nlq) REAL n1,n2,n3,n4 dimension x1(nlq),x2(nlq),x3(nlq),x4(nlq) dimension y1(nlq),y2(nlq),y3(nlq),y4(nlq) dimension z1(nlq),z2(nlq),z3(nlq),z4(nlq) APPENDIX C dimension thick(nlq) dimension thck1(nlq),thck2(nlq),thck3(nlq),thck4(nlq) dimension xdof(nlq,8,3) dimension fx1(nlq),fx2(nlq),fx3(nlq),fx4(nlq) dimension fy1(nlq),fy2(nlq),fy3(nlq),fy4(nlq) dimension fz1(nlq),fz2(nlq),fz3(nlq),fz4(nlq) dimension gl11(nlq),gl21(nlq),gl31(nlq), . gl12(nlq),gl22(nlq),gl32(nlq), . gl13(nlq),gl23(nlq),gl33(nlq) c do i=lft,llt c gmtrx(i,1,1)= 1 x1(i)*dn1dxi+x2(i)*dn2dxi+ 2 x3(i)*dn3dxi+x4(i)*dn4dxi gmtrx(i,2,1)= 1 y1(i)*dn1dxi+y2(i)*dn2dxi+ 2 y3(i)*dn3dxi+y4(i)*dn4dxi gmtrx(i,3,1)= 1 0. gmtrx(i,1,2)= 1 x1(i)*dn1deta+x2(i)*dn2deta+ 2 x3(i)*dn3deta+x4(i)*dn4deta gmtrx(i,2,2)= 1 y1(i)*dn1deta+y2(i)*dn2deta+ 2 y3(i)*dn3deta+y4(i)*dn4deta gmtrx(i,3,2)= 1 0. gmtrx(i,1,3)= 1 0. gmtrx(i,2,3)= 1 0. gmtrx(i,3,3)= 1 .5*thick(i) c coef=.5*thick(i)*zeta c bmtrx(i,1,1,1) =dn1dxi bmtrx(i,1,1,7) =dn2dxi bmtrx(i,1,1,13)=dn3dxi bmtrx(i,1,1,19)=dn4dxi c bmtrx(i,1,1,5) =coef*dn1dxi bmtrx(i,1,1,11)=coef*dn2dxi bmtrx(i,1,1,17)=coef*dn3dxi bmtrx(i,1,1,23)=coef*dn4dxi c bmtrx(i,1,2,1) =dn1deta bmtrx(i,1,2,7) =dn2deta bmtrx(i,1,2,13)=dn3deta bmtrx(i,1,2,19)=dn4deta c bmtrx(i,1,2,5) =coef*dn1deta bmtrx(i,1,2,11)=coef*dn2deta bmtrx(i,1,2,17)=coef*dn3deta bmtrx(i,1,2,23)=coef*dn4deta c bmtrx(i,2,1,2) =dn1dxi bmtrx(i,2,1,8) =dn2dxi bmtrx(i,2,1,14)=dn3dxi bmtrx(i,2,1,20)=dn4dxi c bmtrx(i,2,1,4) =-coef*dn1dxi bmtrx(i,2,1,10)=-coef*dn2dxi bmtrx(i,2,1,16)=-coef*dn3dxi bmtrx(i,2,1,22)=-coef*dn4dxi APPENDIX C c bmtrx(i,1,3,5) =.5*thick(i)*n1 bmtrx(i,1,3,11)=.5*thick(i)*n2 bmtrx(i,1,3,17)=.5*thick(i)*n3 bmtrx(i,1,3,23)=.5*thick(i)*n4 c bmtrx(i,3,1,3) =dn1dxi bmtrx(i,3,1,9) =dn2dxi bmtrx(i,3,1,15)=dn3dxi bmtrx(i,3,1,21)=dn4dxi c bmtrx(i,2,2,2) =dn1deta bmtrx(i,2,2,8) =dn2deta bmtrx(i,2,2,14)=dn3deta bmtrx(i,2,2,20)=dn4deta c bmtrx(i,2,2,4) =-coef*dn1deta bmtrx(i,2,2,10)=-coef*dn2deta bmtrx(i,2,2,16)=-coef*dn3deta bmtrx(i,2,2,22)=-coef*dn4deta c bmtrx(i,2,3,4) =-.5*thick(i)*n1 bmtrx(i,2,3,10)=-.5*thick(i)*n2 bmtrx(i,2,3,16)=-.5*thick(i)*n3 bmtrx(i,2,3,22)=-.5*thick(i)*n4 c bmtrx(i,3,2,3) =dn1deta bmtrx(i,3,2,9) =dn2deta bmtrx(i,3,2,15)=dn3deta bmtrx(i,3,2,21)=dn4deta c enddo c return end To use the element for a part the section card can be written as *SECTION_SHELL $ SECID ELFORM 1 101 $ T1 T2 T3 T4 $ NIPP NXDOF IUNF IHGF 1 0 0 1 $ XI ETA WGT 0. 0. 4. Sample User Solid Element 101 (constant stress solid) The geometry for the constant stress solid is given as 𝑥𝑖 = 𝑥𝑖𝐼𝑁𝐼(𝜉1, 𝜉2) 𝑣𝑖 = 𝑣𝑖𝐼𝑁𝐼(𝜉1, 𝜉2) where, 𝑥𝑖𝐼 = 𝑖th component of coordinate of node 𝐼 𝑣𝑖𝐼 = 𝑖th component of translational velocity of node 𝐼 𝑁𝐼 = shape function localized at node 𝐼 APPENDIX C The matrices necessary for implementing this element as a user-defined solid are derived from the expressions given by and, ∂𝑥𝑖 ∂𝜉1 ∂𝑥𝑖 ∂𝜉2 ∂𝑥𝑖 ∂𝜉3 ∂𝑣𝑖 ∂𝜉1 ∂𝑣𝑖 ∂𝜉2 ∂𝑣𝑖 ∂𝜉3 = 𝑥𝑖𝐼 = 𝑥𝑖𝐼 = 𝑥𝑖𝐼 = 𝑣𝑖𝐼 = 𝑣𝑖𝐼 = 𝑣𝑖𝐼 ∂𝑁𝐼 ∂𝜉1 ∂𝑁𝐼 ∂𝜉2 ∂𝑁𝐼 ∂𝜉3 ∂𝑁𝐼 ∂𝜉1 ∂𝑁𝐼 ∂𝜉2 ∂𝑁𝐼 ∂𝜉3 The user element implementation is given by subroutine usld_b101(bmtrx,gmtrx,gjac, 1 xi,eta,zeta, 2 n1,n2,n3,n4,n5,n6,n7,n8, 3 dn1dxi,dn2dxi,dn3dxi,dn4dxi, 4 dn5dxi,dn6dxi,dn7dxi,dn8dxi, 5 dn1deta,dn2deta,dn3deta,dn4deta, 6 dn5deta,dn6deta,dn7deta,dn8deta, 7 dn1dzeta,dn2dzeta,dn3dzeta,dn4dzeta, 8 dn5dzeta,dn6dzeta,dn7dzeta,dn8dzeta, 9 x1,x2,x3,x4,x5,x6,x7,x8, . y1,y2,y3,y4,y5,y6,y7,y8, . z1,z2,z3,z4,z5,z6,z7,z8, . xdof, . lft,llt) include 'nlqparm' c c Compute b and g matrix for user-defined solid 101 c dimension bmtrx(nlq,3,3,*),gmtrx(nlq,3,3),gjac(nlq) REAL n1,n2,n3,n4,n5,n6,n7,n8 dimension x1(nlq),x2(nlq),x3(nlq),x4(nlq) dimension x5(nlq),x6(nlq),x7(nlq),x8(nlq) dimension y1(nlq),y2(nlq),y3(nlq),y4(nlq) dimension y5(nlq),y6(nlq),y7(nlq),y8(nlq) dimension z1(nlq),z2(nlq),z3(nlq),z4(nlq) dimension z5(nlq),z6(nlq),z7(nlq),z8(nlq) dimension xdof(nlq,8,3) c do i=lft,llt c gmtrx(i,1,1)=x1(i)*dn1dxi+x2(i)*dn2dxi+ 1 x3(i)*dn3dxi+x4(i)*dn4dxi+ APPENDIX C 2 x5(i)*dn5dxi+x6(i)*dn6dxi+ 3 x7(i)*dn7dxi+x8(i)*dn8dxi gmtrx(i,2,1)=y1(i)*dn1dxi+y2(i)*dn2dxi+ 1 y3(i)*dn3dxi+y4(i)*dn4dxi+ 2 y5(i)*dn5dxi+y6(i)*dn6dxi+ 3 y7(i)*dn7dxi+y8(i)*dn8dxi gmtrx(i,3,1)=z1(i)*dn1dxi+z2(i)*dn2dxi+ 1 z3(i)*dn3dxi+z4(i)*dn4dxi+ 2 z5(i)*dn5dxi+z6(i)*dn6dxi+ 3 z7(i)*dn7dxi+z8(i)*dn8dxi gmtrx(i,1,2)=x1(i)*dn1deta+x2(i)*dn2deta+ 1 x3(i)*dn3deta+x4(i)*dn4deta+ 2 x5(i)*dn5deta+x6(i)*dn6deta+ 3 x7(i)*dn7deta+x8(i)*dn8deta gmtrx(i,2,2)=y1(i)*dn1deta+y2(i)*dn2deta+ 1 y3(i)*dn3deta+y4(i)*dn4deta+ 2 y5(i)*dn5deta+y6(i)*dn6deta+ 3 y7(i)*dn7deta+y8(i)*dn8deta gmtrx(i,3,2)=z1(i)*dn1deta+z2(i)*dn2deta+ 1 z3(i)*dn3deta+z4(i)*dn4deta+ 2 z5(i)*dn5deta+z6(i)*dn6deta+ 3 z7(i)*dn7deta+z8(i)*dn8deta gmtrx(i,1,3)=x1(i)*dn1dzeta+x2(i)*dn2dzeta+ 1 x3(i)*dn3dzeta+x4(i)*dn4dzeta+ 2 x5(i)*dn5dzeta+x6(i)*dn6dzeta+ 3 x7(i)*dn7dzeta+x8(i)*dn8dzeta gmtrx(i,2,3)=y1(i)*dn1dzeta+y2(i)*dn2dzeta+ 1 y3(i)*dn3dzeta+y4(i)*dn4dzeta+ 2 y5(i)*dn5dzeta+y6(i)*dn6dzeta+ 3 y7(i)*dn7dzeta+y8(i)*dn8dzeta gmtrx(i,3,3)=z1(i)*dn1dzeta+z2(i)*dn2dzeta+ 1 z3(i)*dn3dzeta+z4(i)*dn4dzeta+ 2 z5(i)*dn5dzeta+z6(i)*dn6dzeta+ 3 z7(i)*dn7dzeta+z8(i)*dn8dzeta c bmtrx(i,1,1,1) =dn1dxi bmtrx(i,1,1,4) =dn2dxi bmtrx(i,1,1,7) =dn3dxi bmtrx(i,1,1,10)=dn4dxi bmtrx(i,1,1,13)=dn5dxi bmtrx(i,1,1,16)=dn6dxi bmtrx(i,1,1,19)=dn7dxi bmtrx(i,1,1,22)=dn8dxi c bmtrx(i,2,1,2) =dn1dxi bmtrx(i,2,1,5) =dn2dxi bmtrx(i,2,1,8) =dn3dxi bmtrx(i,2,1,11)=dn4dxi bmtrx(i,2,1,14)=dn5dxi bmtrx(i,2,1,17)=dn6dxi bmtrx(i,2,1,20)=dn7dxi bmtrx(i,2,1,23)=dn8dxi c bmtrx(i,3,1,3) =dn1dxi bmtrx(i,3,1,6) =dn2dxi bmtrx(i,3,1,9) =dn3dxi bmtrx(i,3,1,12)=dn4dxi bmtrx(i,3,1,15)=dn5dxi bmtrx(i,3,1,18)=dn6dxi bmtrx(i,3,1,21)=dn7dxi bmtrx(i,3,1,24)=dn8dxi c bmtrx(i,1,2,1) =dn1deta bmtrx(i,1,2,4) =dn2deta bmtrx(i,1,2,7) =dn3deta bmtrx(i,1,2,10)=dn4deta APPENDIX C bmtrx(i,1,2,13)=dn5deta bmtrx(i,1,2,16)=dn6deta bmtrx(i,1,2,19)=dn7deta bmtrx(i,1,2,22)=dn8deta c bmtrx(i,2,2,2) =dn1deta bmtrx(i,2,2,5) =dn2deta bmtrx(i,2,2,8) =dn3deta bmtrx(i,2,2,11)=dn4deta bmtrx(i,2,2,14)=dn5deta bmtrx(i,2,2,17)=dn6deta bmtrx(i,2,2,20)=dn7deta bmtrx(i,2,2,23)=dn8deta c bmtrx(i,3,2,3) =dn1deta bmtrx(i,3,2,6) =dn2deta bmtrx(i,3,2,9) =dn3deta bmtrx(i,3,2,12)=dn4deta bmtrx(i,3,2,15)=dn5deta bmtrx(i,3,2,18)=dn6deta bmtrx(i,3,2,21)=dn7deta bmtrx(i,3,2,24)=dn8deta c bmtrx(i,1,3,1) =dn1dzeta bmtrx(i,1,3,4) =dn2dzeta bmtrx(i,1,3,7) =dn3dzeta bmtrx(i,1,3,10)=dn4dzeta bmtrx(i,1,3,13)=dn5dzeta bmtrx(i,1,3,16)=dn6dzeta bmtrx(i,1,3,19)=dn7dzeta bmtrx(i,1,3,22)=dn8dzeta c bmtrx(i,2,3,2) =dn1dzeta bmtrx(i,2,3,5) =dn2dzeta bmtrx(i,2,3,8) =dn3dzeta bmtrx(i,2,3,11)=dn4dzeta bmtrx(i,2,3,14)=dn5dzeta bmtrx(i,2,3,17)=dn6dzeta bmtrx(i,2,3,20)=dn7dzeta bmtrx(i,2,3,23)=dn8dzeta c bmtrx(i,3,3,3) =dn1dzeta bmtrx(i,3,3,6) =dn2dzeta bmtrx(i,3,3,9) =dn3dzeta bmtrx(i,3,3,12)=dn4dzeta bmtrx(i,3,3,15)=dn5dzeta bmtrx(i,3,3,18)=dn6dzeta bmtrx(i,3,3,21)=dn7dzeta bmtrx(i,3,3,24)=dn8dzeta c enddo c return end To use the element for a part the section card can be written as *SECTION_SOLID $ SECID ELFORM 1 101 $ NIP NXDOF IHGF 1 0 1 $ XI ETA ZETA WGT 0. 0. 0. 8.0 APPENDIX C Examples We present three test examples. One example was a simple tension-compression test of a solid cylinder. The geometry is shown in Figure 46-1. The problem is using the sample implementations of user elements and compared the results and performance with standard LS-DYNA elements. As for the computational efficiency, we note that the performance is worse but this is expected since there is little room for optimization of the code while retaining a user friendly interface. The implicit performance compares well with the other elements in LS-DYNA. The second example was a combined bending and stretching example with the geometry shown in Figure 46-2. Again we ran the problem with the user element implementations and compared the results and performance with standard LS-DYNA elements. We could see the same tendencies as for the solid elements. The third and final example is an impact between a solid bar and shell beam. Both parts are modeled with user-defined elements. The results were very similar to the ones obtained by substituting the sections for standard LS-DYNA sections, but the simulation time was about 3-4 times longer. APPENDIX C Figure 46-1. Solid mesh for user element test. Figure 46-2. Shell mesh for the user element test. APPENDIX C Figure 46-3. Impact between a user-defined shell and user-defined solid part. APPENDIX D APPENDIX D: User Defined Airbag Sensor The addition of a user sensor subroutine into LS-DYNA is relatively simple. The sensor is mounted on a rigid body which is attached to the structure. The motion of the sensor is provided in the local coordinate system defined for the rigid body in the definition of material model 20–the rigid material. When the user defined criterion is met for the deployment of the airbag, a flag is set and the deployment begins. All load curves relating to the mass flow rate versus time are then shifted by the initiation time. The user subroutine is given below with all the necessary information contained in the comment cards. subroutine airusr (rbu,rbv,rba,time,dt1,dt2,param,hist,itrnon, . rbug,rbvg,rbag,icnv) c c****************************************************************** c| Livermore Software Technology Corporation (LSTC) | c| ------------------------------------------------------------ | c| Copyright 1987-2008 Livermore Software Tech. Corp | c| All rights reserved | c****************************************************************** c c user subroutine to initiate the inflation of the airbag c c variables c c displacements are defined at time n+1 in local system c velocites are defined at time n+1/2 in local system c accelerations are defined at time n in local system c c rbu(1-3) total displacements in the local xyz directions c rbu(3-6) total rotations about the local xyz axes c rbv(1-3) velocities in the local xyz directions c rbv(3-6) rotational velocities about the local xyz axes c rba(1-3) accelerations in the local xyz directions c rba(3-6) rotational accelerations about the local xyz axes c time is the current time c dt1 is time step size at n-1/2 c dt2 is time step size at n+1/2 c param is user defined input parameters c hist is user defined history variables c itrnon is a flag to turn on the airbag inflation c rbug,rbvg,rbag, are similar to rbu,rbv,rba but are defined c globally. c icnv is the airbag ID c c the user subroutine sets the variable itrnon to: c c itrnon=0 bag is not inflated c itrnon=1 bag inflation begins and this subroutine is c not called again c include 'iounits.inc' dimension rbu(6),rbv(6),rba(6),param(25),hist(25), . rbug(6),rbvg(6),rbag(6) c itrnon=0 ra=sqrt(rba(1)**2+rba(2)**2+rba(3)**2) if (ra.gt.param(1)) then APPENDIX D itrnon=1 write(iotty,100) time write(iohsp,100) time write(iomsg,100) time endif 100 format (' Airbag activated at time ',1pe10.3) c return end APPENDIX E APPENDIX E: User Defined Solution Control This subroutine may be provided by the user to control the I/O, monitor the energies and other solution norms of interest, and to shut down the problem whenever he pleases. The arguments are defined in the listing provided below. This subroutine is called each time step and does not need any control card to operate. subroutine uctrl1 (numnp,ndof,time,dt1,dt2,prtc,pltc,frci,prto, . plto,frco,vt,vr,at,ar,ut,ur,xmst,xmsr,irbody,rbdyn,usrhv, . messag,totalm,cycle,idrint,mtype,mxrb,nrba,rbcor,x,rbv,nrbn, . nrb,xrb,yrb,zrb,axrb,ayrb,azrb,dtx,nmmat,rba,fvalnew,fvalold, . fvalmid,fvalnxt) c c****************************************************************** c| Livermore Software Technology Corporation (LSTC) | c| ------------------------------------------------------------ | c| Copyright 1987-2008 Livermore Software Tech. Corp | c| All rights reserved | c****************************************************************** c c user subroutine for solution control and is called at the c beginning of time step n+1. The time at n+ c c c note: ls-dyna3d uses an internal numbering system to c accomodate arbitrary node numbering. to access c information for user node n, address array location m, c m = lqf8(n,1). to obtain user node number, n, c corresponding to array address m, set n = lqfinv(m,1) c c arguments: c numnp = number of nodal points c ndof = number of degrees of freedom per node c time = current solution time at n+1 c dt1 = time step size between time n-1 and n c dt2 = time step size between time n and n+1 c prtc = output interval for taurus time history data c pltc = output interval for taurus state data c frci = output interval for taurus interface force data c prto = output time for time history file c plto = output time for state data c frco = output time for force data c vt(3,numnp) = nodal translational velocity vector c vr(3,numnp) = nodal rotational velocity vector. this c array is defined if and only if ndof = 6 c at(3,numnp) = nodal translational acceleration vector c ar(3,numnp) = nodal rotational acceleration vector. this c array is defined if and only if ndof = 6 c ut(3,numnp) = nodal translational displacement vector c ur(3,numnp) = nodal rotational displacement vector. this c array is defined if and only if ndof = 6 c xmst(numnp) = reciprocal of nodal translational masses c xmsr(numnp) = reciprocal of nodal rotational masses. this c array is defined if and only if ndof = 6 APPENDIX E c fvalold = array for storing load curve values at time n c fvalnew = array for setting load curve values at time n+1 c only load curves with 0 input points may be user c defined. When the load curve is user set, the c value at time n must be stored in array fvalold. c fvalmid = array for predicting load curve values at time n+3/2 c fvalnxt = array for predicting load curve values at time n+2 c for some applications it is necessary to predict the c load curve values at time n+2, a time that is not known, c this for instance for boundary prescribed motion. In c this case the load curve values at time n+3/2 need to c be predicted in fvalmid, and fvalold should be set to c fvalnew and fvalnew should be set to fvalnxt. See c coding below. c c irbody = 0 if no rigid bodies c rbdyn(numnp)=flag for rigid body nodal points c if deformable node then set to 1.0 c if rigid body node then set to 0.0 c defined if and only if rigid bodies are present c i.e., irbody.ne.0 if no rigid bodies are c present c usrhv(lenhv)=user defined history variables that are stored c in the restart file. lenhv = 100+7*nummat where c nummat is the # of materials in the problem. c array usrhv is updated only in this subroutine. c messag = flag for dyna3d which may be set to: c 'sw1.' ls-dyna3d terminates with restart file c 'sw3.' ls-dyna3d writes a restart file c 'sw4.' ls-dyna3d writes a plot state c totalm = total mass in problem c cycle = cycle number c idrint = flag for dynamic relaxation phase c .ne.0: dynamic relaxation in progress c .eq.0: solution phase c include 'ptimes.inc' c c prtims(1-37)=output intervals for ascii files c c ascii files: c ( 1)-cross section forces c ( 2)-rigid wall forces c ( 3)-nodal data c ( 4)-element data c ( 5)-global data c ( 6)-discrete elements c ( 7)-material energies c ( 8)-noda interface forces c ( 9)-resultant interface forces c (10)-smug animator c (11)-spc reaction forces c (12)-nodal constraint resultant forces c (13)-airbag statistics c (14)-avs database c (15)-nodal force groups c (16)-output intervals for nodal boundary conditions c (17)-(32) unused at this time c (37)-auto tiebreak damage output APPENDIX E c c prtlst(32)=output times for ascii files above. when solution time c exceeds the output time a print state is dumped. c common/rbkeng/enrbdy,rbdyx,rbdyy,rbdyz c c total rigid body energies and momentums: c enrbdy = rigid body kinetic energy c rbdyx = rigid body x-momentum c rbdyy = rigid body y-momentum c rbdyz = rigid body z-momentum c common/swmke/swxmom,swymom,swzmom,swkeng c c total stonewall energies and momentums: c swxmom = stonewall x-momentum c swymom = stonewall y-momentum c swzmom = stonewall z-momentum c swkeng = stonewall kinetic energy c common/deengs/deeng c c deeng = total discrete element energy c common/bk28/summss,xke,xpe,tt,xte0,erodeke,erodeie,selie,selke, . erodehg c c xpe = total internal energy in the finite elements c common/sprengs/spreng c c spreng = total spr energy c character*(*) messag integer cycle real*8 x dimension vt(3,*),vr(3,*),at(3,*),ar(3,*), . xmst(*),xmsr(*),rbdyn(*),usrhv(*),mtype(*),mxrb(*),nrba(*), . rbcor(3,1),x(*),rbv(6,*),nrbn(*),nrb(*),xrb(*),yrb(*), . zrb(*),axrb(*),ayrb(*),azrb(*),rba(6,*),fvalnew(*), . fvalold(*),fvalmid(*),fvalnxt(*) real*8 ut(3,*),ur(3,*) c c sample momentum and kinetic energy calculations c c remove all comments in column 1 below to activate i = 1 if (i.eq.1) return c return cc cc cc initialize kinetic energy, xke, and x,y,z momentums. cc c xke = 2.*swkeng+2.*enrbdy c xm = swxmom+rbdyx c ym = swymom+rbdyy c zm = swzmom+rbdyz cc c numnp2 = numnp c if (ndof.eq.6) then APPENDIX E c numnp2 = numnp+numnp c endif c write(iotty,*)ndof cc cc cc no rigid bodies present cc c if (irbody.eq.0) then cc note in blank comment vr follows vt. this fact is used below. c do 10 n = 1,numnp2 c xmsn = 1./xmst(n) c vn1 = vt(1,n) c vn2 = vt(2,n) c vn3 = vt(3,n) c xm = xm+xmsn*vn1 c ym = ym+xmsn*vn2 c zm = zm+xmsn*vn3 c xke = xke+xmsn*(vn1*vn1+vn2*vn2+vn3*vn3) c 10 continue cc cc cc rigid bodies present cc c else cc nodal accerations for rigid bodies cc c do 12 n = 1,nmmat c if (mtype(n).ne.20.or.mxrb(n).ne.n) go to 12 c lrbn = nrba(n) c call stvlut(rbcor(1,n),x,vt,at,ar,vr,rbv(1,n),dt2, c . nrbn(n),nrb(lrbn),xrb,yrb,zrb,axrb,ayrb,azrb,dtx) c c rigid body nodal accelerations c c if (ndof.eq.6) then c call rbnacc(nrbn(n),nrb(lrbn),rba(4,n),ar) c endif c c 12 continue cc c do 20 n = 1,numnp c xmsn = 1./xmst(n) c vn1 = rbdyn(n)*vt(1,n) c vn2 = rbdyn(n)*vt(2,n) c vn3 = rbdyn(n)*vt(3,n) c xm = xm+xmsn*vn1 c ym = ym+xmsn*vn2 c zm = zm+xmsn*vn3 c xke = xke+xmsn*(vn1*vn1+vn2*vn2+vn3*vn3) c 20 continue c if (ndof.eq.6) then c do 30 n = 1,numnp c xmsn = 1./xmsr(n) c vn1 = rbdyn(n)*vr(1,n) c vn2 = rbdyn(n)*vr(2,n) c vn3 = rbdyn(n)*vr(3,n) c xm = xm+xmsn*vn1 c ym = ym+xmsn*vn2 c zm = zm+xmsn*vn3 c xke = xke+xmsn*(vn1*vn1+vn2*vn2+vn3*vn3) APPENDIX E c 30 continue c endif c endif cc cc total kinetic energy c xke=.5*xke cc total internal energy c xie = xpe+deeng+spreng cc total energy c xte = xke+xpe+deeng+spreng cc total x-rigid body velocity c xrbv = xm/totalm cc total y-rigid body velocity c yrbv = ym/totalm cc total z-rigid body velocity c zrbv = zm/totalm return end APPENDIX F APPENDIX F: User Defined Interface Control This subroutine may be provided by the user to turn the interfaces on and off. This option is activated by the *USER_INTERFACE_CONTROL keyword. The arguments are defined in the listing provided below. subroutine uctrl2(nsi,nty,time,cycle,msr,nmn,nsv,nsn, 1 thmr,thsv,vt,xi,ut,iskip,idrint,numnp,dt2,ninput,ua, 2 irectm,nrtm,irects,nrts) c c****************************************************************** c| Livermore Software Technology Corporation (LSTC) | c| ------------------------------------------------------------ | c| Copyright 1987-2008 Livermore Software Tech. Corp | c| All rights reserved | c****************************************************************** c c user subroutine for interface control c c note: ls-dyna3d uses an internal numbering system to c accomodate arbitrary node numbering. to access c information for user node n, address array location m, c m = lqf8(n,1). to obtain user node number, n, c corresponding to array address m, set n = lqfinv(m,1) c c arguments: c nsi = number of sliding interface c nty = interface type. c .eq.4:single surface c .ne.4:surface to surface c time = current solution time c cycle = cycle number c msr(nmn) = list of master nodes numbers in internal c numbering scheme c nmn = number of master nodes c nsv(nsn) = list of slave nodes numbers in internal c numbering scheme c nsn = number of slave nodes c thmr(nmn) = master node thickness c thsv(nsn) = slave node thickness c vt(3,numnp)=nodal translational velocity vector c xi(3,numnp)=initial coordinates at time = 0 c ut(3,numnp)=nodal translational displacement vector c idrint = flag for dynamic relaxation phase c .ne.0: dynamic relaxation in progress c .eq.0: solution phase c numnp = number of nodal points c dt2 = time step size at n+1/2 c ninput = number of variables input into ua c ua(*) = users' array, first ninput locations c defined by user. the length of this c array is defined on control card 10. c this array is unique to interface nsi. c irectm(4,*)=list of master segments in internal APPENDIX F c numbering scheme c nrtm = number of master segments c irects(4,*)=list of slave segments in internal c numbering scheme c nrts = number of master segments c c set flag for active contact c iskip = 0 active c iskip = 1 inactive c c******************************************************************* c integer cycle real*8 ut real*8 xi dimension msr(*),nsv(*),thmr(*),thsv(*),vt(3,*),xi(3,*), . ut(3,*),ua(*),irectm(4,*),irects(4,*) c c the following sample of codeing is provided to illustrate how c this subroutine might be used. here we check to see if the c surfaces in the surface to surface contact are separated. if c so the iskip = 1 and the contact treatment is skipped. c c if (nty.eq.4) return c dt2hlf = dt2/2. c xmins = 1.e+16 c xmaxs = -xmins c ymins = 1.e+16 c ymaxs = -ymins c zmins = 1.e+16 c zmaxs = -zmins c xminm = 1.e+16 c xmaxm = -xminm c yminm = 1.e+16 c ymaxm = -yminm c zminm = 1.e+16 c zmaxm = -zminm c thks = 0.0 c thkm = 0.0 c do 10 i = 1,nsn c dsp1 = ut(1,nsv(i))+dt2hlf*vt(1,nsv(i)) c dsp2 = ut(2,nsv(i))+dt2hlf*vt(2,nsv(i)) c dsp3 = ut(3,nsv(i))+dt2hlf*vt(3,nsv(i)) c x1 = xi(1,nsv(i))+dsp1 c x2 = xi(2,nsv(i))+dsp2 c x3 = xi(3,nsv(i))+dsp3 c thks = max(thsv(i),thks) c xmins = min(xmins,x1) c xmaxs = max(xmaxs,x1) c ymins = min(ymins,x2) c ymaxs = max(ymaxs,x2) c zmins = min(zmins,x3) c zmaxs = max(zmaxs,x3) c 10 continue c do 20 i = 1,nmn c dsp1 = ut(1,msr(i))+dt2hlf*vt(1,msr(i)) c dsp2 = ut(2,msr(i))+dt2hlf*vt(2,msr(i)) c dsp3 = ut(3,msr(i))+dt2hlf*vt(3,msr(i)) c x1 = xi(1,msr(i))+dsp1 c x2 = xi(2,msr(i))+dsp2 APPENDIX F c x3 = xi(3,msr(i))+dsp3 c thkm = max(thmr(i),thks) c xminm = min(xminm,x1) c xmaxm = max(xmaxm,x1) c yminm = min(yminm,x2) c ymaxm = max(ymaxm,x2) c zminm = min(zminm,x3) c zmaxm = max(zmaxm,x3) c 20 continue c c if thks or thkm equal zero set them to some reasonable value c c if (thks.eq.0.0) then c e1=(xi(1,irects(1,1))-xi(1,irects(3,1)))**2 c . +(xi(2,irects(1,1))-xi(2,irects(3,1)))**2 c . +(xi(3,irects(1,1))-xi(3,irects(3,1)))**2 c e2=(xi(1,irects(2,1))-xi(1,irects(4,1)))**2 c . +(xi(2,irects(2,1))-xi(2,irects(4,1)))**2 c . +(xi(3,irects(2,1))-xi(3,irects(4,1)))**2 c thks=.3*sqrt(max(e1,e2)) c endif c if (thkm.eq.0.0) then c e1=(xi(1,irectm(1,1))-xi(1,irectm(3,1)))**2 c . +(xi(2,irectm(1,1))-xi(2,irectm(3,1)))**2 c . +(xi(3,irectm(1,1))-xi(3,irectm(3,1)))**2 c e2=(xi(1,irectm(2,1))-xi(1,irectm(4,1)))**2 c . +(xi(2,irectm(2,1))-xi(2,irectm(4,1)))**2 c . +(xi(3,irectm(2,1))-xi(3,irectm(4,1)))**2 c thkm=.3*sqrt(max(e1,e2)) c endif c c if (xmaxs+thks.lt.xminm-thkm) go to 40 c if (ymaxs+thks.lt.yminm-thkm) go to 40 c if (zmaxs+thks.lt.zminm-thkm) go to 40 c if (xmaxm+thkm.lt.xmins-thks) go to 40 c if (ymaxm+thkm.lt.ymins-thks) go to 40 c if (zmaxm+thkm.lt.zmins-thks) go to 40 c iskip = 0 c c return c 40 iskip = 1 c return end APPENDIX G APPENDIX G: User Defined Interface Friction and Conductivity An easy-to-use user contact interface is provided in LS-DYNA where the user has the possibility to define the frictional coefficients (static and dynamic) as well as contact heat transfer conductance as functions of contact pressure, relative sliding velocity, separation and temperature. To be able to use this feature, an object version of the LS- DYNA code is required and the user must write his/her own Fortran (or C) code to define the contact parameters of interest. In the text file dyn21.f that comes with the object version of LS-DYNA, the subroutines of interest are subroutine usrfrc(fstt,fdyn,...) for defining the frictional coefficients fstt (static) and fdyn (dynamic) and subroutine usrhcon(h,...) for defining the heat transfer contact conductance h. We emphasize at this point that the user friction interface differs between LS-DYNA (SMP) and MPP-DYNA (MPP), for reasons that have to do with how the contacts are implemented in general. In LS-DYNA (SMP) the user is required not only to define the frictional coefficients but also to assemble and store contact forces and history, whereas in MPP-DYNA (MPP) only the frictional coefficients have to be defined. For the friction interface (SMP and MPP) the user may associate history variables with each contact node. Unfortunately, the user friction interface is currently not supported by all available contacts in LS-DYNA and MPP-DYNA, but it should cover the most interesting ones among others, *CONTACT_(FORMING_)NODES_TO_SURFACE, *CONTACT_(FORMING_)SURFACE_TO_SURFACE, *CONTACT_(FORMING_)ONE_ WAY_SURFACE_TO_SURFACE. Upon request by customers additional contact types can be supported. One of the arguments to the user contact routines is the curve array crv, also available in the user material interface. Note that when using this array, the curve identity must be converted to an internal number or the subroutine crvval may be utilized. For more information, see the appendix A on user materials. For definition of user contact parameters the user must define the keywords *USER_INTERFACE_FRICTION or *USER_INTERFACE_CONDUCTIVITY APPENDIX G The card format for these two keywords are identical and can be found in other sections in this manual. There is an alternate route to defining the conductivity parameters for a user defined thermal contact. On the *CONTACT_..._THERMAL_FRICTION optional card the parameter FORMULA may be set to a negative number. This will automatically create a user defined conductivity interface and invoke reading of –FORMULA contact parameters immediately following the card including the FORMULA parameter. Note that FORMULA is related to NOC and NOCI in the *USER_INTERFACE_CONDUC- TIVITY keyword as – FORMULA = NOC = NOCI. Note that the pressure is automatically computed for each user conductivity interface, i.e., the keyword *LOAD_SURFACE_STRESS is not necessary. A sample friction subroutine is provided below for SMP. subroutine usrfrc(nosl,time,ncycle,dt2,insv,areas,xs,ys,zs, . lsv,ix1,ix2,ix3,ix4,aream,xx1,xx2,xx3,stfn,stf,fni, . dx,dy,dz,fdt2,ninput,ua,side,iisv5,niisv5,n1,n2,n3,fric1, . fric2,fric3,fric4,bignum,fdat,iseg,fxis,fyis,fzis,ss,tt, . ilbsv,stfk,frc,numnp,npc,pld,lcfst,lcfdt,temp,temp_bot, . temp_top,isurface) c c****************************************************************** c| LIVERMORE SOFTWARE TECHNOLOGY CORPORATION (LSTC) | c| ------------------------------------------------------------ | c| COPYRIGHT © 1987-2007 JOHN O. HALLQUIST, LSTC | c| ALL RIGHTS RESERVED | c****************************************************************** c c user subroutine for interface friction control c c note: LS-DYNA uses an internal numbering system to c accomodate arbitrary node numbering. to access c information for user node n, address array location m, c m=lqf(n,1). to obtain user node number, n, c corresponding to array address m, set n=lqfinv(m,1) c c arguments: c c nosl =number of sliding interface c time =current solution time c ncycle =ncycle number c dt2 =time step size at n+1/2 c insv =slave node array where the nodes are stored c in ls-dyna3d internal numbering. User numbers c are given by function: lqfinv(insv(ii),1) c for slave node ii. c areas(ii) =slave node area (interface types 5&10 only) for c slave node ii c xs(ii) =x-coordinate slave node ii (projected) c ys(ii) =y-coordinate slave node ii (projected) c zs(ii) =z-coordinate slave node ii (projected) c lsv(ii) =master segment number for slave node ii c ix1(ii), ix2(ii), ix3(ii), ix4(ii) c =master segment nodes in ls-dyna3d internal c numbering for slave node ii APPENDIX G c aream(ii) =master segment area for slave node ii. c xx1(ii,4) =x-coordinates master surface (projected) for c slave node ii c xx2(ii,4) =y-coordinates master surface (projected) for c slave node ii c xx3(ii,4) =z-coordinates master surface (projected) for c slave node ii c stfn =slave node penalty stiffness c stf =master segment penalty stiffness c fni =normal force c dx,dy,dz =relative x,y,z-displacement between slave node and c master surface. Multipling by fdt2 defines the c relative velocity. c n1,n2,n3 =x,y, and z components of master segments normal c vector c c*********************************************************************** c frictional coefficients defined for the contact interface c c fric1 =static friction coefficient c fric2 =dynamic friction coefficient c fric3 =decay constant c fric4 =viscous friction coefficient (setting fric4=0 c turns this option off) c c*********************************************************************** c c bignum =0.0 for one way surface to surface and c for surface to surface, and 1.e+10 for nodes c to surface contact c ninput =number of variables input into ua c ua(*) =users' array, first ninput locations c defined by user. the length of this c array is defined on control card 10. c this array is unique to interface nosl. c c side ='master' for first pass. the master c surface is the surface designated in the c input c ='slave' for second pass after slave and c master surfaces have be switched for c the type 3 symmetric interface treatment. c c iisv5 =an array giving the pointers to the active nodes c in the arrays. c c niisv5 =number of active nodes c c fdat =contact history data array c iseg =contact master segment from previous step. c fxis =slave node force component in global x dir. c to be updated to include friction c fyis =slave node force component in global y dir. c to be updated to include friction c fzis =slave node force component in global z dir. c to be updated to include friction c ss(ii) =s contact point (-1 to 1) in parametric coordinates c for slave node ii. c tt(ii) =t contact point (-1 to 1) in parametric coordinates c for slave node ii. c ilbsv(ii) =pointer for node ii into global arrays. c stfk(ii) =penalty stiffness for slave node ii which was used c to compute normal interface force. c frc(1,lsv(ii)) c =Coulomb friction scale factor for segment lsv(ii) c frc(2,lsv(ii)) APPENDIX G c =viscous friction scale factor for segment lsv(ii) c c*********************************************************************** c parameters for a coupled thermal-mechanical contact c c numnp = number of nodal points in the model c npc = load curve pointer c pld = load curve (x,y) data c lcfst(nosl)= load curve number for static coefficient of c friction versus temperture for contact c surface nosl c lcfdt(nosl)= load curve number for dynamic coefficient of c friction versus temperture for contact c surface nosl c temp(j) = temperature for node point j c temp_bot(j)= temparature for thick thermal shell bottom c surface c temp_top(j)= temparature for thick thermal shell top c surface c numsh12 = number of thick thermal shells c itopaz(1) = 999 ==> thermal-mechanical analysis c isurface = thick thermal shell surface pointer c c*********************************************************************** APPENDIX H APPENDIX H: User Defined Thermal Material Model The addition of a thermal user material routine into LS-DYNA is fairly straightforward. The thermal user material is controlled using the keyword *MAT_THERMAL_USER_- DEFINED, which is described at the appropriate place in the manual. The thermal user material can be used alone or in conjunction with any given mechanical material model in a coupled thermal-mechanical solution. A heat-source can be included and the specific heat updated so that it possible to model e.g. phase transformations including melt energy. If for the same part (shell or solid elements) both a thermal and mechanical user material model is defined then the two user material models have (optionally) read access to each other’s history variables. If the integration points of the thermal and mechanical elements not are coincident then interpolation or extrapolation is used when reading history variables. Linear interpolation or extrapolation using history data from the two closest integration points is used in all cases except when reading history variables from the thick thermal shell (THSHEL = 1 on *CONTROL_SHELL). For the latter thermal shell, the shape functions of the element are used for the interpolation or extrapolation. The thermal user materials are thermal material types 11-15. These thermal user material subroutines are defined in file dyn21.f as subroutines thumat11, … , thumat15. The latter subroutines are called from the subroutine thusrmat. The source code of subroutine thusrmat is also in file dyn21.f. Additional useful information is available in the comments of subroutines thusrmat, thumat12, and umat46 that all reside in the source file dyn21.f Thermal history variables Thermal history variables can be used by setting NVH greater that 0. Thermal history variables are output to the tprint file, see *DATABASE_TPRINT. Interchange of history variables with mechanical user material In a coupled thermo-mechanical solution there is for each mechanical shell, thick shell, or solid element a corresponding thermal element. A pair consisting of a mechanical and a corresponding thermal element both have integration points and possibly history variables. The mechanical and thermal elements do not necessarily have the same number of integration points. APPENDIX H By setting IHVE to 1, a thermal user material model can read, but not write, the history variables from a mechanical user material model and vice versa. If the locations of the points where the history variables are located differ between the mechanical and thermal element differ interpolation or extrapolation is used to calculate the history value. More information is available in the comments to the subroutines thusrmat and thumat11. Limitations: Currently there are a few limitations of the thermal user material implementation. LS- DYNA will in most cases give an appropriate warning or error message when such a limit is violated. The limitations include: 1. Option IHVE.EQ.1 is only supported for a limited range of mechanical elements: a) Solid elements: ELFORM = 1, 2, 10, 13. b) Shell elements: ELFORM = 2, 3, 4, 16. Note that user-defined integration rules are not supported. 2. Thermal history variables limitations: a) Thermal history variables are not output to d3plot. 3. The thermal solver includes not only the plastically dissipated energy as a heat source but also wrongly the elastic energy. The latter however is in most cases not of practical importance. Example source code: Example source code for thermal user material models is available in thumat11 and thumat12 as well as in umat46. Note that there is space for up to 64 material parameters in r_matp (material parameter array) but only 32 can be read in from the *MAT_THER- MAL_USER_DEFINED card. The material parameters in r_matp(i), i = 41-64, which are initially set to 0.0, may be used by the user to store additional data. Subroutine crvval evaluates load curves. Note that when using crvval the load curves are first re-interpolated to 100 equidistant points. See Appendix A for more information on subroutine crvval. Following is a short thermal user material model. The card format is in this case, if enabling orthotropic conduction, and with sample input in SI-units: Card 1 1 Variable MID 2 RO 3 MT 4 5 6 7 8 LMC NVH AOPT IORTHO IHVE Type 21 7800.0 12.0 6.0 3.0 0.0 1.0 0.0 Card 2 Variable 1 XP 2 YP 3 ZP 4 A1 5 A2 6 A3 7 8 Type 0.0 0.0 0.0 0.0 0.0 0.0 Card 3 Variable 1 D1 2 D2 3 D3 Type 0.0 0.0 0.0 4 5 6 7 8 Card 4 Variable 1 C1 2 C2 3 C3 4 HC 5 6 7 8 HSRC HCFAC Type 25.0 25.0 20.0 470.0 11.0 12.0 VARIABLE DESCRIPTION C1-C3 HC HSRC Heat conduction in 11, 22, and 33 direction of material coordinate system. Heat capacity Load curve ID of load curve giving a heat source output (W/m3) as a function of time. HCFAC Load curve ID of load curve giving a scaling of the heat capacity as function of time. APPENDIX H The source code is: subroutine thumat12(c1,c2,c3,cvl,dcvdtl,hsrcl,dhsrcdtl, 1 hsv,hsvm,nmecon,r_matp,crv, 2 nel,nep,iep,eltype,dt,atime,ihsrcl) character*(*) eltype dimension hsv(*),hsvm(*),r_matp(*),crv(101,2,*) include 'iounits.inc' c c Thermal user-material number 12. c c See comments at the beginning of subroutine thusrmat c for instructions. c c Example: isotropic/orthotropic material with k1=P1 and c cvl=P2 for solid and shell elements including optional c change of heat capacity and a heat source, both functions c of time input as load curves. c c Print out some info on start-up, use material parameter 64 c as a flag. if(nint(r_matp(64)).eq.0) then r_matp(64)=1. write( *,1200) (r_matp(8+i),i=1,6) write(iohsp,1200) (r_matp(8+i),i=1,6) write(59,1200) (r_matp(8+i),i=1,6) endif c c Calculate response c1=r_matp(8+1) c2=r_matp(8+2) c3=r_matp(8+3) cvl=r_matp(8+4) dcvdtl=0.0 eid=nint(r_matp(8+6)) if(nint(eid).gt.0) then call crvval(crv,eid,atime,cvlfac,tmp1) cvl=cvl*cvlfac dcvdtl=0.0 endif c c If flux or time step calculation then we are done. if(eltype.eq.'soliddt'.or.eltype.eq.'flux'.or. . eltype.eq.'shelldt') return eid=nint(r_matp(8+5)) if(nint(eid).gt.0) then ihsrcl=1 call crvval(crv,eid,atime,hsrcl,tmp1) dhsrcdtl=0.0 endif c c Update history variables hsv(1)=cvl hsv(2)=atime hsv(3)=hsv(3)+1.0 c c Done return 1200 format(/'This is thermal user defined material #12. '/ 1 /' Material parameter c1-c3 : ',3E10.3 2 /' Material parameter hc : ',E10.3 3 /' Heat source load curve : ',F10.0 4 /' hc scale factor load curve : ',F10.0 5 /' Thermal History variable 1 : cv' 6 /' Thermal History variable 2-3 : Dummy'/) return end APPENDIX H APPENDIX I APPENDIX I: Occupant Simulation Including the Coupling to the CAL3D and MADYMO programs INTRODUCTION LS-DYNA is coupled to occupant simulation codes to generate solutions in automotive crashworthiness that include occupants interacting with the automotive structure. In such applications LS-DYNA provides the simulation of the structural and deformable aspects of the model and the OSP (Occupant Simulation Program) simulates the motion of the occupant. There is some overlap between the two programs which provides flexibility in the modeling approach. For example, both the OSP and LS-DYNA have the capability of modeling seat belts and other deformable restraints. The advantage of using the OSP is related to the considerable databases and expertise that have been developed in the past for simulating dummy behavior using these programs. The development of the interface provided LSTC a number of possible approaches. The approach selected is consistent with the LSTC philosophy of providing the most flexible and useful interface possible. This is important because the field of non-linear mechanics is evolving rapidly and techniques which are used today are frequently rendered obsolete by improved methodologies and lower cost computing which allows more rigorous techniques to be used. This does make the learning somewhat more difficult as there is not any single procedure for performing a coupling. One characteristic of LS-DYNA is the large number of capabilities, particularly those associated with rigid bodies. This creates both an opportunity and a difficulty: LS- DYNA3D has many ways approximating different aspects of problems, but they are frequently not obvious to users without considerable experience. Therefore, in this Appendix we emphasize modeling methods rather than simply listing capabilities. THE LS-DYNA/OCCUPANT SIMULATION PROGRAM LINK Coupling between the OSP and LS-DYNA is performed by combining the programs into a single executable. In the case of CAL3D, LS-DYNA calls CAL3D as a subroutine, but in the case of MADYMO, LS-DYNA is called as a subroutine. The two programs are then integrated in parallel with the results being passed between the two until a user defined termination time is reached. The OSP and LS-DYNA have different approaches to the time integration schemes. The OSP time integrators are based on accurate implicit integrators which are valid for large time steps which are on the order of a millisecond for the particular applications of APPENDIX I interest here. An iterative solution is used to insure that the problem remains in equilibrium. The implicit integrators are extremely good for smoothly varying loads, however, sharp nonlinear pulses can introduce considerable error. An automatic time step size control which decreases the time step size quickly restores the accuracy for such events. The LS-DYNA time integrator is based on an explicit central difference scheme. Stability requires that the time step size be less than the highest frequency in the system. For a coarse airbag mesh, this number is on the order of 100 microseconds while an actual car crash simulation is on the order of 1 microsecond. The smallest LS- DYNA models have at least 1,000 elements. Experience indicates that the cost of a single LS-DYNA time step for a small model is at least as great as the cost of a time step in the OSP. Therefore, in the coupling, the LS-DYNA time step is used to control the entire simulation including the OSP part. This approach has negligible cost penalties and avoids questions of stability and accuracy that would result by using a subcycling scheme between the two programs. LS-DYNA has a highly developed rigid body capability which is used in different parts of automobile crash simulation. In particular, components such as the engine are routinely modeled with rigid bodies. These rigid bodies have been modified so that they form the basis of the coupling procedure in LS-DYNA to the OSP. Please contact the LSTC technical support team (support@lstc.com) for instructions to download and run LS-DYNA executables coupled with Madymo. AIRBAG MODELING Modeling of airbags is accomplished by use of shell or membrane elements in conjunction with a control volume and possibly a single surface contact algorithm to eliminate interpenetrations during the inflation phase . The contact types showing an “a” in front are most suited for airbag analysis. Current recommended material types for the airbags are: 1. 2. 3. *MAT_ELASTIC (Type 1, Elastic) *MAT_COMPOSITE_DAMAGE (Type 22, layered orthotropic elastic for composites) *MAT_FABRIC (Type 34, fabric model for folded airbags) Model 34 is a “fabric” model which can be used for flat bags. As a user option this model may or may not support compression. The elements which can be used are as follows: 1. Belytschko-Tsay quadrilateral with 1 point quadrature. This element behaves rather well for folded and unfolded cases with only a small tendency to hour- APPENDIX I glass. The element tends to be a little stiff. Stiffness form hourglass control is recommended. 2. Belytschko-Tsay membrane. This model is softer than the normal Belytschko- Tsay element and can hourglass quite badly. Stiffness form hourglass is rec- ommended. As a better option, the fully integrated Belytschko-Tsay membrane element can be chosen. 3. C0 Triangular element. The C0 triangle is very good for flat bag inflation and has no tendency to hourglass. 4. The best choice is a specially developed airbag membrane element with quadrilateral shape. This is an automatic choice when the fabric material is used. As an airbag inflates, a considerable amount of energy is transferred to the surrounding air. This energy transfer decreases the kinetic energy of the bag as it inflates. In the control volume logic, this is simulated either by using either a mass weighted damping option or a back pressure on the bag based on a stagnation pressure. In both cases, the energy that is absorbed is a function of the fabric velocity relative to a rigid body velocity for the bag. For the mass weighted case, the damping force on a node is proportional to the mass times the damping factor times the velocity vector. This is quite effective in maintaining a stable system, but has little physical justification. The latter approach using the stagnation pressure method estimates the pressure needed to accelerate the surrounding air to the speed of the fabric. The formula for this is: 𝑃 = Area × 𝛼 × [(𝑉⃗⃗⃗⃗⃗𝑖 − 𝑉⃗⃗⃗⃗⃗𝑐𝑔) ⋅ 𝑛̂] This formula accomplishes a similar function and has a physical justification. Values of the damping factor, 𝛼, are limited to the range of 0 to 1, but a value of 0.1 or less is more likely to be a good value. COMMON ERRORS 1. Improper airbag inflation or no inflation. The most common problem is inconsistency in the units used for the input constants. An inflation load curve must also be specified. The normals for the airbag segments must all be consistent and facing outwards. If a negative vol- ume results, this can sometimes be quickly cured by using the “flip” flag on the control volume definition to force inward facing normals to face outwards. 2. Excessive airbag distortions. Check the material constants. Triangular elements should have less distortion problems than quadrilaterals. Overlapped elements at time zero can cause APPENDIX I locking to occur in the contact leading to excessive distortions. The considera- ble energy input to the bag will create numerical noise and some damping is recommended to avoid problems. 3. The dummy passes through the airbag. A most likely problem is that the contacts are improperly defined. Another possibility is that the models were developed in an incompatible unit system. The extra check for penetration flag if set to 1 on the contact control cards vari- able PENCHK in the *CONTACT_... definitions may sometimes cause nodes to be prematurely released due to the softness of the penalties. In this case the flag should be turned off. 4. The OSP fails to converge. This may occur when excessively large forces are passed to the OSP. First, check that unit systems are consistent and then look for improperly defined contacts in the LS-DYNA input. 5. Time step approaches zero. This is almost always in the airbag. If elastic or orthotropic (*MAT_ELASTIC or *MAT_COMPOSITE material 1 or 22) is being used, then switch to fabric mate- rial *MAT_FABRIC which is less time step size sensitive and use the fully inte- grated membrane element. Increasing the damping in the control volume usually helps considerably. Also, check for “cuts” in the airbag where nodes are not merged. These can allow elements to deform freely and cut the time step to zero. APPENDIX J APPENDIX J: Interactive Graphics Commands Only the first four or less characters of command are significant. These commands are available in the interactive phase of LS-DYNA. The interactive graphics are available by using the “SW5.” command after invoking the Ctrl-C interrupt. The MENU command brings up a push button menu. Only available in Unix and Linux. ANIMATE Animate saved sequence, stop with switch 1. BACK BGC BIP CENTER CL CMA COLOR Return to previous display size after zoom, then list display attributes. Change display background color RGB proportions BGC <red> <green> <blue>. Select beam integration point for contour; BIP <#>. Center model, center on node, or center with mouse, i.e., center cent <value> or cent gin. Classification labels on display; class commercial_in_ confidence. Color materials on limited color displays. Set or unset shaded coloring of materials. CONTOUR View with colored contour lines; contour < component #> < list mat #>; see TAURUS manual. COOR COP CR CUT CX CY CZ Get node information with mouse. Hardcopy of display on the PC copy < laserj paintj tekcol coljet or epson>. Restores cutting plane to default position. Cut away model outside of zoom window; use mouse to set zoom window size. Rotate slice plane at zmin about x axis. Rotate slice plane at zmin about y axis. Rotate slice plane at zmin about z axis. APPENDIX J DIF DISTANCE Change diffused light level for material; DIF < mat #, -1 for all > <value>. Set distance of model from viewer; DIST < value in normalized model dimensions>. DMATERIALS Delete display of material DMAT < ALL or list of numbers>. in subsequent views; DRAW DSCALE DYN ELPLT END ESCAPE EXECUTE FCL FOV FRINGE Display outside edges of model. Scale current displacement from initial shape. After using TAURUS command will reset display to read current DYNA3D state data. Set or unset element numbering in subsequent views. Delete display and return to execution. Escapes from menu pad mode. Return to execution and keep display active. Fix or unfix current contour levels. Set display field of view angle; FOV < value in degrees>. View with colored contour fringes; fringe < component #> < list mat #>; see TAURUS manual. GETFRAME Display a saved frame; GETF < frame #>. HARDWARE Hardware mode; workstation hardware calls are used to draw, move and color model; repeat command to reset to normal mode. HELP HZB LIMIT MAT Switch on or off hardware zbuffer for a subsequent view, draw or contour command; rotations and translations will be in hardware. Set range of node numbers subsequent views; limit < first node #> < last node #>. Re-enable display of deleted materials mat < all or list of numbers>. MENU MOTION MOV NDPLT APPENDIX J Button menu pad mode. Motion of model through mouse movement or use of a dial box. The left button down enables translation in the plane, middle button rotation about axes in the plane; and with right button down in the out of plane axis; left and middle button down quit this mode. Drag picked part to new position set with mouse. Set or unset node numbering in subsequent views. NOFRAME Set and unset drawing of a frame around the picture. PAUSE Animation display pause in seconds PHS2 or THISTORY Time history plotting phase. Similar to LS-TAURUS. PICK POST QUIT RANGE RAX RAY RAZ RESTORE Get element information with mouse. Enable or disable postscript mode on the PC and eps file is written as picture is drawn; remove eofs and init- graphics for eps use. Same as execute. Set fix range for contour levels; range <minvalue> <maxvalue>. Reflect model about xy plane; restore command will switch-off reflections. Reflect model about yz plane; restore command will switch-off reflections. Reflect model about zx plane, restore command will switch-off reflections. Restores model to original position, also switches off element and node numbers, slice capper, reflections and cut model. RETURN Exit. RGB RX Change color red green blue element < mat #> <red> <green> <blue>. Rotate model about x axis. APPENDIX J RY RZ SAVE SEQUENCE SHR SIP SLICE SNORMAL SPOT TAURUS TRIAD TSHELL TV TX TY TZ V VECTOR v or d ZB ZIN Rotate model about y axis. Rotate model about z axis. Set or unset saving of display for animation. Periodic plot during execution; SEQ <# of cy- cles > <commands> EXE. Shrink element facets towards centroids in subsequent views, shrink <value>. Select shell integration point for contour; SIP <#>. Slice model a z-minimum plane; slice < value in normalized model dimension > this feature is removed after using restore. Slice enables internal details for brick elements to be used to generate new polygons on the slice plane. Set or unset display of shell direction normals to indicate topology order. Draw node numbers on model spot < first #> < last # for range>. LS-DYNA database, TAU < state #>, or state < state #>, reads LS-TAURUS file to extract previous state data. Set or unset display of axis triad. Set or unset shell element thickness simulation in subsequent views. Change display type. Translates model along x axis. Translates model along y axis. Translates model along z axis. Display model using painters algorithm. View with vector arrows of velocity or displacement; <v> or <d>. Switch on or off zbuffer algorithm for subsequent view; or draw commands. Zoom in using mouse to set display size and position. ZMA ZMI ZOUT APPENDIX J Set position of zmax plane; ZMAX < value in normalized model dimensions>. Set position of zmin plane; ZMIN < value in normalized model dimensions>. Zoom out using mouse to set displays size expansion and position. APPENDIX K APPENDIX K: Interactive Material Model Driver INTRODUCTION The interactive material model driver in LS-DYNA allows calculation of the material constitutive response to a specified strain path. Since the constitutive model subroutines in LS-DYNA are directly called by this driver, the behavior of the constitutive model is precisely that which can be expected in actual applications. In the current implementation the constitutive subroutines for both shell elements and solid elements can be examined. INPUT DEFINITION The material model driver is invoked when no *NODE or *ELEMENT commands are present in a standard LS-DYNA input file. The number of material model definitions should be set to one, the number of load curves should be nine, and the termination time to the desired length of the driver run. The complete state dump interval as given in *DATABASE_BINARY_D3PLOT serves as the time step to be used in the material model driver run. Plotting information is saved in core for the interactive plotting phase. The input deck typically consists only of *KEYWORD, *DATABASE_BINARY_D3PLOT, *CONTROL_TERMINATION, one each of *PART/*MAT/*SECTION, and nine load curves (*DEFINE_CURVE) describing the strain path. These nine curves define the time history of the displacement gradient components shown in Table 54-1. The velocity gradient matrix, Lij, is approximated by taking the time derivative of the components in Table 54-1. If these components are considered to form a tensor Sij , then 𝐿𝑖𝑗(𝑡) = 𝑆𝑖𝑗(𝑡) − 𝑆𝑖𝑗(𝑡𝑘−1) (𝑡 − 𝑡𝑘) and the strain rate tensor is defined as and the spin tensor as 𝑑𝑖𝑗 = 𝐿𝑖𝑗 + 𝐿𝑖𝑗 𝜔𝑖𝑗 = 𝐿𝑖𝑗 − 𝐿𝑖𝑗 APPENDIX K Load Curve Number Component Definition 1 2 3 4 5 6 7 8 9 ∂𝑢 ∂𝑥 ∂𝑣 ∂𝑦 ∂𝑤 ∂𝑧 ∂𝑢 ∂𝑦 ∂𝑣 ∂𝑥 ∂𝑢 ∂𝑧 ∂𝑤 ∂𝑥 ∂𝑣 ∂𝑧 ∂𝑤 ∂𝑦 Table 54-1. Load Curve Definitions versus Time INTERACTIVE DRIVER COMMANDS After reading the input file and completing the calculations, LS-DYNA gives a command prompt to the terminal. A summary of the available interactive commands is given below. An on-line help package is available by typing HELP. Only available in Unix and Linux. ACCL Scale all abscissa data by f. Default is f = 1. ASET amin omax Set min and max values on abscissa to amin and amax, respectively. If amin = amax = 0, scaling is automatic. CHGL n Change prompts for new label. label for component n. LS-DYNA APPENDIX K CONTINUE Re-analyze material model. CROSS c1 c2 Plot component c1 versus c2. ECOMP Display component numbers on the graphics dis- play: EQ.1: x-stress, EQ.2: y-stress, EQ.3: z-stress, EQ.4: xy-stress, EQ.5: yz-stress, EQ.6: zx-stress, EQ.7: effective plastic strain, EQ.8: pressure, EQ.9: von Mises (effective) stress, EQ.10: 1st principal deviatoric stress, EQ.11: 2nd principal deviatoric stress, EQ.12: 3rd principal deviatoric stress, EQ.13: maximum shear stress, EQ.14: 1st principal stress, EQ.15: 2nd principal stress, EQ.16: 3rd principal stress, EQ.17: ln (v ⁄ v0), EQ.18: relative volume, EQ.19: v0 ⁄ v - 1.0, EQ.20: 1st history variable, EQ.21: 2nd history variable. Adding 100 or 400 to component numbers 1-16 yields strains and strain rates, respectively. FILE name Change pampers filename to name for printing. GRID NOGRID Graphics displays will be overlaid by a grid of or- thogonal lines. Graphics displays will not be overlaid by a grid of orthogonal lines. OSCL Scale all ordinate data by f. Default is f = 1. OSET omin omax Set min and max values on ordinate to omin and omax, respectively. If omin = omax = 0, scaling is automatic. APPENDIX K PRINT Print plotted time history data into file “pampers.” Only data plotted after this command is printed. File name can be changed with the “file” com- mand. QUIT, END, T Exit the material model driver program. RDLC m n r1 z1 ... rn zn Redefine load curve m using n coordinate pairs (r1,z1) (r2,z2),...(rn,zn). TIME c TV n Plot component c versus time. Use terminal output device type n. LS-DYNA provides a list of available devices. Presently, the material model drive is implemented for solid and shell element material models. The driver does not yet support material models for beam elements. Use the keyword *CONTROL_MPP_MATERIAL_MODEL_DRIVER and run the input deck only on one processor if a distributed memory executable (MPP) is used. APPENDIX L APPENDIX L: VDA Database VDA surfaces describe the surface of geometric entities and are useful for the simulation of sheet forming problems. The German automobile and automotive supplier industry (VDA) has defined the VDA guidelines [VDA 1987] for a proper surface definition used for the exchange of surface data information. In LS-DYNA, this format can be read and used directly. Some files have to be provided for proper linkage to the motion of the correlation parts/materials in LS-DYNA. Linking is performed via names. To these names surfaces are attached, which in turn can be linked together from many files externally to LS-DYNA. Thus, arbitrary surfaces can be provided by a preprocessor and then can be written to various files. The so- called VDA file given on the LS-DYNA execution line via V = vda contains references to all other files. It also contains several other parameters affecting the treatment in the contact subroutines; see below. The procedure is as follows. If VDA surfaces are to be used, the file specified by vda must have the following form. The file is free formatted with blanks as delimiters. Note that the characters “}” and “{” must be separated from the other input by spaces or new lines. The vda file may contain any number of input file specifications of the form: file afile bfile { alias definitions } alias definitions followed by optional runtime parameters and a final end statement. The file, afile, is optional, and if given must be the name of an ASCII input file formatted in accordance with the VDA Surface Interface Definitions as defined by the German automobile and automotive supply industry. bfile is required, and is the name of a binary VDA file. In a first run afile is given and bfile is created. In any further run, if the definitions have not changed, afile can be dropped and only bfile is needed. The purpose of bfile is that it allows for much faster initialization if the same VDA surfaces are to be used in a future LS-DYNA run. If afile is given, bfile will always be created or overwritten. The alias definitions are used for linking to LS-DYNA and between the various surface definitions in the files defined by afile and bfile. The alias definitions are of the form alias name { el1 el2 ... eln } where name is any string of up to 12 characters, and el1,...,eln are the names of VDA elements as specified in afile. The list of elements can be empty, in which case all the SURF and FACE VDA elements in afile will be used. Care should be taken to ensure that the alias name is unique, not only among the other aliases, but among the VDA APPENDIX L offset 10 5 0 0 1 goffset alias die 1 2 1 5 0 0 1 { previous alias dieold } vw die P = (1,2,1) zoffset = 1 woffset = 5 element 10 (a) zoffset = 1 poffset = 5 dieold (b) Figure 55-1. (a) a schematic illustration of offset version 1, and (b) is a schematic illustration of offset version 2. element names in afile. This collection of VDA elements can later be indicated by the alias name. In particular, name may appear in later alias definitions. Often it is required that a punch or die be created by a simple offset. This can be achieved in the vda files in two ways, either on VDA elements directly, or on parts defined by aliases. This feature offers great capability in generating and using surface data information. Offset Version 1 As an option, the keyword offset may appear in the alias list which allows a new surface to be created as a normal offset (plus translation) of a VDA element in the file. The keyword offset my be applied to VDA elements only, not aliases. The usage of offset follows the form offset elem normal x y z where normal is the amount to offset the surface along the normal direction, and x,y,z are the translations to be applied. The default normal direction is given by the cross product of the local u and v directions on the VDA surface, taken in that order. normal can be negative. Offset Version 2 Frequently, it is convenient to create a new alias name by offsetting and translating an existing name. The keyword goffset provides this function: goffset alias name xc yc zc normal x y z { previous alias name } where normal, x, y, and z are defined as in the offset keyword. A reference point xc, yc, and zc defines a point in space which determines the normal direction to the VDA surface, which is a vector from the origin to P(xc,yc,zc). See example below. APPENDIX L Finally, several parameters affecting the VDA surface iteration routines can be reset in the file vda. These parameters, and their default values in square brackets [ ], are: gap [5.0] track [2.0] track2 [5.0] ntrack [4] The maximum allowable surface gap to be filled in during the iterations. Points following the surface will effectively extend the edg- es of surfaces if necessary to keep them from falling through cracks in the surface smaller than this. This number should be set as small as possible while still allowing correct results. In particular, if your VDA surfaces are well formed (having no gaps), this parameter can be set to 0.0. The default value is 5.0. A point must be within this distance of contact to be continually tracked. When a point not being tracked comes close to a surface, a global search is performed to find the near surface point. While a point is being tracked, iterations are performed every cycle. These iterations are much faster, but if the point is far away it is faster to occasionally do the global search. The default value is 2.0. Every VDA surface is surrounded by a bounding box. When a global search needs to be performed but the distance from a point to this box is > track2, the actual global search is not performed. This will require another global search to be performed sooner than if the actual distance to the surface were known, but also allows many global searches to be skipped. The default value is 5.0. The number of VDA surfaces for which each point maintains actual distance information. A global lower bound on distance is maintained for all remaining surfaces. Whenever the point moves far enough to vi- olate this global lower bound, all VDA surfaces must have the global search performed for them. Hence, this parameter should be set to the maximum number of surfaces that any point can be expected to be near at one time (the largest number of surfaces that come together at one point). Setting ntrack higher will require more memory but result in faster execution. If ntrack is too low, performance may be unacceptably slow. The default value is 4.0. APPENDIX L toroid [.01] Any surface with opposing edges which are within distance [t] of each other is assumed to be cylindrical. Contacts occurring on one edge can pass to the adjacent edge. The default value is 0.01. converge [.01] When surface iterations are performed to locate the near point, iteration is continued until convergence is detected to within this distance (all VDA coordinates are in mm). The default value is 0.01. iterate [8] Maximum number of surface iterations allowed. Since points being tracked are checked every cycle, if convergence fails it will be tried again next cycle, so setting this parameter high does not necessarily help much. On the other hand, a point converging to a crease in the VDA surface (a crease between patches with discontinuous derivative, for example) may bounce back and forth between patches up to this many times, without actually moving. Hence, this value should not be too large. The default value is 8. el_size [t mx mn] Controls the generation of elements where: t = surface tolerance for mesh generation, mx = maximum element size to generate, mn = minimum element size to generate. The default values are [0.25 100. 1.0] aspect [s1 s2] Controls the generation of elements where: s1 = maximum difference in aspect ratio between elements generated in neighboring VDA patches, s2 = maximum aspect ratio for any generated element. The default values are [1.5 4.0] cp_space [10] Determines the spacing around the boundaries of parts at which the size of elements is controlled. In the interior of the part, the element size is a weighted function of these control points as well as additional control points in the interior of the region. If there are too few control points around the boundary, elements generated along or near straight boundaries, but between control points, may be too small. The default value is 10. meshonly The existence of this keyword causes LS-DYNA to generate a file containing the mesh for the VDA surfaces and then terminate. onepatch The existence of this keyword causes LS-DYNA to generate a single element on each VDA patch. somepatch [n] Like onepatch, but generates an element for 1 out of every [n] patches. Example for file V = vda. It contains the following data: APPENDIX L file vda1 vda1.bin { alias die { sur0001 sur0003 offset fce0006 1.5 0 0 120 } alias holder1 { sur008 } } file vda2 vda2.bin { alias holder2 { sur003 } } alias holder { holder1 holder2 } ntrack 6 gap 0.5 end Explanation: vda1 This file contains the surfaces/face elements sur0001,sur0003, fce0006, and sur0008. alias die face Combines the surface/face elements sur0001, sur0003, and the offsetted fce0006 to a global surface. alias holder1 Defines the surface/face element sur0008 as holder1. vda2 This file contains the surface/face element sur0003. alias holder2 Defines the surface/face element sur0003 as holder2. alias holder Combines the surfaces holder1 and holder2 into a combined surface holder. ntrack 6 For each point the actual distances to 6 VDA surfaces are maintained. gap 0.5 Surface gaps of 0.5mm or less are filled. end Closes reading of this file. APPENDIX M APPENDIX M: Commands for Two-Dimensional Rezoning The rezoner in LS-DYNA contains many commands that can be broken down into the following categories: •general, •termination of interactive rezoning, •redefinition of output intervals for data, •graphics window controls, •graphics window controls for x versus y plots, •mesh display options, •mesh modifications, •boundary modifications, •MAZE line definitions, •calculation graphics display control parameters, •calculation graphics display, •cursor commands. The use of the rezoner is quite simple. Commands for rezoning material number n can be invoked after the material is specified by the “M n” command. To view material n, the command “V” is available. The interior mesh can be smoothed with the “S” command and the boundary nodes can be adjusted after the “B” command is used to display the part side and boundary node numbers. Commands that are available for adjusting boundary nodes following the “B” command include: ER, EZ, ES, VS, BD, ERS, EZS, ESS, VSS, BDS, SLN, SLNS Rezoning is performed material by material. An example is shown. Do not include the graphics display type number when setting up a command file for periodic noninteractive rezoning. No plotting is done when the rezoner is used in this mode. REZONING COMMANDS BY FUNCTION: Interactive Real Time Graphics SEQ n commands EXE Every n time steps execute the graphics commands which follow. For example the line seq 100 g exe would APPENDIX M General C FRAME HELP cause the grid to be updated on the graphics display de- vice every 100 cycles. The real time graphics can be ter- minated by using ctrl-c and typing “sw7.” Comment - proceed to next line. Frame plots with a reference grid (default). Enter HELP package and display all available commands. Description of each command is available in the HELP package. HELP/commandname Do not enter HELP package but print out the description on the terminal of the command following the slash. LOGO NOFRAME PHP ans RESO nx ny TV n TR t Put LLNL logo on all plots (default). Retyping this command removes the logo. Do not plot a reference grid. Print help package - If answer equals ‘y’ the package is printed in the high speed printer file. Set the x and y resolutions of plots to nx and ny, respectively. We default both nx and ny to 1024. Use graphics output device type n. The types are installation dependent and a list will be provided after this command is invoked. At time t, LS-DYNA will stop and enter interactive rezoning phase. Termination of Interactive Rezoning F FR Terminate execution phase. interactive phase, remap, continue in Terminate interactive phase, remap, write restart dump, and call exit. T or END Terminate. APPENDIX M Redefinition of Output Intervals for Data PLTI t PRTI t TERM t Reset the node and element data dump interval t. Reset the node and element printout interval t. Reset the termination to t. Graphics Window Controls ESET n FF FIX FSET n r z GSET r z l GRID NOGRID SETF r z r z UNFIX UZ a b l Center picture at element n with a r by z window. This window is set until it is released by the unfix command or reset with another window. Encircle picture with reference grid with tickmarks. Default grid is plotted along bottom and left side of pic- ture. Set the display to its current window. This window is set until it is reset by the “GSET, “FSET”, or “SETF” com- mands or released by the “UNFIX” command. Center display at node n with a rectangular Δ𝑟 × Δ𝑧 window. This window is set until it is reset with or the “UNFIX” command is typed. Center display picture at point (r,z) with square window of width l. This window is set until it is reset or the “UNFIX” command is typed. Overlay graphics displays with a grid of orthogonal lines. Do not overlay graphics displays with a grid of orthogonal lines (default). Center display at point (r,z) with a rectangular Δ𝑟 × Δ𝑧 window. This window is set until it is reset or the “UN- FIX” command is typed. Release current display window set by the “FIX”, “GSET”, “FSET” or “SETF” commands. Zoom in at point (a,b) with window l where a, b, and l are numbers between 0 and 1. The picture is assumed to lie in a unit square. APPENDIX M UZG UZOU a b l Z r z l∆ ZOUT r z l∆ Cover currently displayed picture with a 10 by 10 square grid to aid in zooming with the unity zoom, “UZ”, com- mand. Zoom out at point (a,b) with window l where a, b, and l are numbers between 0 and 1. The current window is scaled by the factor 1 ∆⁄ l.The picture is assumed to lie in a unit square. Zoom in at point (r,z) with window ∆l. ∆ ∆ Zoom out at point (r,z) with window l. The window is enlarged by the ratio of the current window and l. The cursor may be used to zoom out via the cursor command DZOU and entering two points with the cursor to define the window. The ratio of the current window with the specified window determines the picture size reduction. An alternative cursor command, DZZO, may be used and only needs one point to be entered at the location where the reduction (2×) is expected. Graphics Window Controls for x versus y plots The following commands apply to line plots, interface plots, etc. ASCL fa Scale all abscissa data by fa. The default is fa = 1. ASET amin amax Set minimum and maximum values on abscissa to amin and amax, respectively. If amin = amax = 0.0 (default) LS-DYNA determines the minimum and maximum val- ues. OSCL fo Scale all ordinate data by fo. The default is fo = 1. OSET omin omax Set minimum and maximum values on ordinate to omin and omax, respectively. If omin = omax = 0.0 (default) LS-DYNA determines the minimum and maximum val- ues. SMOOTH n Smooth a data curve by replacing each data point by the average of the 2n adjacent points. The default is n = 0. Mesh Display Options ELPLT Plot element numbers on mesh of material n. FSOFF FSON G GO GS M n MNOFF MNON NDPLT O RPHA RPVA TN r z l UG V VSF APPENDIX M Turn off the “FSON” command. Plot only free surfaces and slideline interfaces with “O” command. (Must be used before “O” command.) View mesh. View mesh right of centerline and outline left of centerline. View mesh and solid fill elements to identify materials by color. Material n is to be rezoned. Do not plot material numbers with the “O”, “G”, and “GO” commands (default). Plot material numbers with “O”, “G”, and “GO” commands. Plot node numbers on mesh of material n. Plot outlines of all material. Reflect mesh, contour, fringe, etc., plots about horizontal axis. Retyping “RPHA” turns this option off. Reflect mesh, contour, fringe, etc., plots about vertical axis. Retyping “RPVA” turns this option off. Type node numbers and coordinates of all nodes within window (r ± ∆l⁄2, z ± ∆l⁄2). Display undeformed mesh. Display material n on graphics display. See command M. Display material n on graphics display and solid fill elements. Mesh Modifications BACKUP Restore mesh to its previous state. This command undoes the result of the last command. APPENDIX M BLEN s Smooth option where s = 0 and s = 1 correspond to equipotential and isoparametric smoothing, respectively. By letting 0 ≤ s ≤ 1 a combined blending is obtained. CN m r z Node m has new coordinate (r,z). DEB n f1 l1 ... fn ln Delete n element blocks consisting of element numbers f1 to l1, f2 to l2 ... , and fo ln inclusive. These elements will be inactive when the calculation resume. DE e1 e2 Delete elements e1 to e2. DMB n m1 m2 ... mn Delete n material blocks consisting of all elements with material numbers m1, m2,..., and mn. These materials will be inactive when the calculations resume. DM n m1 m2 ... mn Delete n materials including m1, m2,..., and mn. DZER k d incr nrow Delete element row where k is the kept element, d is the deleted element, incr is the increment, and nrow is the number of elements in the row. DZLN number n1 n2 n3...nlast Delete nodal row where number is the number of nodes in the row and n1, n2, ... nlast are the ordered list of delet- ed nodes. DZNR l j incr Delete nodal row where l is the first node in the row, j is the last node in the row, and incr is the increment. R S Restore original mesh. Smooth mesh of material n. To smooth a subset of elements, a window can be set via the “GSET”, “FSET”, OR “SETF” commands. Only the elements lying within the window are smoothed. Boundary Modifications A B BD m n 56-6 (APPENDIX M) Display all slidelines. Slave sides are plotted as dashed lines. Determine boundary nodes and sides of material n and display boundary with nodes and side numbers. Dekink boundary from boundary node m to boundary BDS s Dekink side s. DSL n l1 l2...ln Delete n slidelines including slideline numbers l1 l2..., and ln. APPENDIX M ER m n ERS s ES m n ESS s EZ m n EZS s MC n MD n MN n SC n SD n SLN m n SLNS n SN n Equal space in r-direction boundary nodes m to n (counterclockwise). Equal space in the r-direction boundary nodes on side s. Equal space along boundary, boundary nodes m to n (counterclockwise). Equal space along boundary, boundary nodes on side s. Equal space in z-direction boundary nodes m to n (counterclockwise). Equal space in the z-direction boundary nodes on side s. Check master nodes of slideline n and put any nodes that have penetrated through the slave surface back on the slave surface. Dekink master side of slideline n. After using this command, the SC or MC command is sometimes advisa- ble. Display slideline n with master node numbers. Check slave nodes of slideline n and put any nodes that have penetrated through the master surface back on the master surface. Dekink slave side of slideline n; after using this command, the SC or MC command is sometimes advisa- ble. Equal space boundary nodes between nodes m to n on a straight line connecting node m to n. Equal space boundary nodes along side n on a straight line connecting the corner nodes. Display slideline n with slave node numbers. APPENDIX M VS m n r VSS s r MAZE Line Definitions B LD n k l LDS n l M n Vary the spacing of boundary nodes m to n such that r is the ratio of the first segment length to the last segment length. Vary the spacing of boundary nodes on side s such that r is the ratio of the first segment length to the last segment length. Determine boundary nodes and sides of material n and display boundary with nodes and side numbers. See command “M”. Line definition n for MAZE includes boundary nodes k to l Line definition n for MAZE consists of side number l. Material n is active for the boundary command B. Calculation Graphics Display Control Parameters MOLP Overlay the mesh on the contour, fringe, principal stress, and principal strain plots. Retyping “MOLP” turns this option off. NLOC Do not plot letters on contour lines. NUMCON n Plot n contour levels. The default is 9. PLOC RANGE r1 r2 Plot letters on contour lines to identify their levels (default). Set the range of levels to be between r1 and r2 instead of in the range chosen automatically by LS-DYNA. To de- activate this command, type RANGE 0 0. Calculation Graphics Display CONTOUR c n m1 m2...mn Contour component number c on n materials including materials m1, m2, ..., mn. If n is zero, only the outline of material m1 with contours is plotted. Component num- bers are given in Table 56-1. FRINGE c n m1 m2...mn IFD n IFN l m IFP c m IFS m IFVA rc zc IFVS LINE c n m1 m2...mn NCOL n NLDF n n1 n2...n3 NSDF m NSSDF l m APPENDIX M Fringe component number c on n materials including m1, m2,...,mn. If n is zero, only the outline of material m1 with contours is plotted. Component numbers are given in Table 56-1. Begin definition of interface n. If interface n has been previously defined, this command has the effect of de- stroying the old definition. Include boundary nodes l to m (counterclockwise) in the interface definition. This command must follow the “B” command. Plot component c of interface m. Component numbers are given in Table 56-2. Include side m in the interface definition. Side m is defined for material n by the “B” command. Plot the angular location of the interface based on the center point (rc,zc) along the abscissa. Positive angles are measured counterclockwise from the y-axis. Plot the distance along the interface from the first interface node along the abscissa (default). Plot variation of component c along line defined with the “NLDF”, “PLDF”, “NSDF”, or the “NSSDF” commands given below. In determining variation, consider n mate- rials including material number m1, m2,...mn. Number of colors in fringe plots is n. The default value for n is 6 which includes colors magenta, blue, cyan, green, yellow, and red. An alternative value for n is 5 which eliminates the minimum value magenta. Define line for “LINE” command using n nodes including node numbers n1, n2,...nn. This line moves with the nodes. Define line for “LINE” command as side m. Side m is defined for material n by the “B” command. Define line for “LINE” command and that includes boundary nodes l to m (counterclockwise) in the interface APPENDIX M definitions. This command must follow the “B” com- mand. PLDF n r1 z1...rn zn Define line for “LINE” command using n coordinate pairs (r1,z1), (r2,z2), ...(rn,zn). This line is fixed in space. PRIN c n m1 m2...mn PROFILE c n m1 m2...mn VECTOR c n m1 m2...mn Plot lines of principal stress and strain in the yz plane on n materials including materials m1, m2,...,mn. If n is zero, only the outline of material m1 is plotted. The lines are plotted in the principal stress and strain directions. Per- missible component numbers in Table M.1 include 0, 5, 6, 100, 105, 106,...,etc. Orthogonal lines of both maximum and minimum stress are plotted if components 0, 100, 200, etc. are specified. Plot component c versus element number for n materials including materials m1, m2,...,mn. If n is 0/ then compo- nent c is plotted for all elements. Component numbers are given in Table M.1. Make a vector plot of component c on n materials including materials m1, m2,...,mn. If n is zero, only the outline of material m1 with vectors is plotted. Compo- nent c may be set to “D” and “V” for vector plots of dis- placement and velocity, respectively. No. Component No. Component APPENDIX M y z hoop yz maximum principal minimum principal von Mises (Appendix A) 21* ln (V⁄Vo) (volumetric strain) 22* y-displacement z-displacement 23* 24* maximum displacement y-velocity, y-heat flux 25* z-velocity, y-heat flux 26* 27* maximum velocity, maximum 1 2 3 4 5 6 7 8 9 28 29 30 31 32 pressure or average strain maximum principal - minimum principal y minus hoop 10 11 maximum shear ij and kl normal 12 jk and li normal ij and kl shear jk and li shear y-deviatoric z-deviatoric hoop-deviatoric effective plastic strain temperature/internal energy density 13 14 15 16 17 18 19* 20* 41*-70* element history variables 71* r-peak acceleration 76* heat flux ij normal jk normal kl normal li normal ij shear jk shear kl shear li shear relative volume V⁄Vo 33 34 35 36* 37* Vo⁄V-1 38* 39* bulk viscosity, Q P + Q 40* density 72* 73* 74* 75* z-peak acceleration r-peak velocity z-peak velocity peak value of max. in plane prin. stress 77* 78* 79* peak value of min in plane prin. stress peak value of maximum hoop stress peak value of minimum hoopstress peak value of pressure Table 56-1. Component numbers for element variables. By adding 100, 200 300, 400, 500 and 600 to the component numbers not followed by an asterisk, component numbers for infinitesimal strains, lagrange strains, almansi strains, strain rates, extensions, and residual strain are obtained. Maximum and minimum principal stresses and strains are in the rz plane. The corresponding hoop quantities must be examined to determine the overall extremum. ij, jk, etc. normal components are normal to the ij, jk, etc side. The peak value database must be flagged on Control Card 4 in columns 6-10 or components 71-79 will not be available for plotting. APPENDIX M No. Component 1 2 3 4 5 6 pressure shear stress normal force tangential force y-force z-force Table 56-2. Component numbers for interface variables. In ax- isymmetric geometries the force is per radian. Cursor Commands DBD a b DCN a b DCSN n a DCNM a b DER a b DES a b DEZ a b DTE a b DTN a b Use cursor to define points a and b on boundary. Dekink boundary starting at a, moving counterclockwise, and end- ing at b. Use cursor to define points a and b. The node closest to point a will be moved to point b. Move nodal point n to point a defined by the cursor. Use cursor to define points a and b. The node at point a is given the coordinate at point b. Use cursor to define points a and b on boundary. Equal space nodes in r-direction along boundary starting at a, moving counterclockwise, and ending at b. Use cursor to define points a and b on boundary. Equal space nodes along boundary starting at a, moving counter- clockwise, and ending at b. Use cursor to define points a and b on boundary. Equal space nodes in z-direction along boundary starting at a, moving counterclockwise, and ending at b. Use cursor to define points a and b on the diagonal of a window. The element numbers and coordinates of ele- ments lying within the window are typed on the terminal. Use cursor to define points a and b on the diagonal of a window. The node numbers and coordinates of nodal points lying within the window are typed on the terminal. DTNC a DVS a b r DZ a b DZOUT a b DZZ a APPENDIX M Use cursor to define point a. The nodal point number and nodal coordinates of the node lying closest to point a will be printed. Use cursor to define points a and b on boundary. Variable space nodes along boundary starting at a, moving counter- wise, and ending at b. The ratio of the first segment length to the last segment length is give by r (via terminal). Use cursor to define points a and b on the diagonal of a window for zooming. Enter two points with the cursor to define the window. The ratio of the current window with the specified window de- termines the picture size reduction. Use cursor to define point a and zoom in at this point. The new window is .15 as large as the previous window. The zoom factor can be reset by the crzf command for the .15 default. DZZO a Zoom out at point a by enlarging the picture two times. APPENDIX N APPENDIX N: Rigid-Body Dummies The two varieties of rigid body dummies available in LS-DYNA are described in this appendix. These are generated internally by including the appropriate *COMPONENT keyword. A description of the GEBOD dummies begins on this page and the HYBRID III family on page N.7. GEBOD Dummies Rigid body dummies can be generated and simulated within LS-DYNA using the keyword *COMPONENT_GEBOD. Physical properties of these dummies draw upon the GEBOD database [Cheng et al. 1994] which represents an extensive measurement program conducted by Wright-Patterson AFB and other agencies. The differential equations governing motion of the dummy are integrated within LS-DYNA separate from the finite element model. Interaction between the dummy and finite element structure is achieved using contact interfaces . neck upper torso middle torso lower torso head right shoulder right upper arm right lower arm right hand right upper right lower leg right foot Figure 57-1. 50th percentile male dummy in the nominal position. APPENDIX N The dynamical system representing a dummy is comprised of fifteen rigid bodies (segments) and include: lower torso, middle torso, upper torso, neck, head, upper arms, forearms/hands, upper legs, lower legs, and feet. Ellipsoids are used for visualization and contact purposes. Shown in Figure 57-1 is a 50th percentile male dummy generated using the keyword command *COMPONENT_GEBOD_MALE. Note that the ellipsoids representing the shoulders are considered to be part of the upper torso segment and the hands are rigidly attached to the forearms. Each of the rigid segments which make up the dummy is connected to its neighbor with a joint which permits various relative motions of the segments. Listed in the Table 57-2 are the joints and their applicable degrees of freedom. Joint Name pelvis waist Degree(s) of Freedom 1st 2nd lateral flexion (x) forward flexion (y) lateral flexion (x) forward flexion (y) lower neck lateral flexion (x) forward flexion (y) upper neck lateral flexion (x) forward flexion (y) 3rd torsion (z) torsion (z) torsion (z) torsion (z) shoulders abduction-adduction (x) internal-external rotation (z) flexion-extension (y) elbows flexion-extension (y) n/a n/a hips abduction-adduction (x) medial-lateral rotation (z) flexion-extension (y) knees flexion-extension (y) n/a n/a ankles inversion-eversion (x) dorsi-plantar flexion (y) medial-lateral rotation (z) Table 57-2. Joints and associated degrees of freedom. Local axes are in parentheses. Orientation of a segment is effected by performing successive right-handed rotations of that segment relative to its parent segment - each rotation corresponds to a joint degree of freedom. These rotations are performed about the local segment axes and the sequence is given in Table 57-2. For example, the left upper leg is connected to the lower torso by the left hip joint; the limb is first abducted relative to lower torso, it then undergoes lateral rotation, followed by extension. The remainder of the lower extremity (lower leg and foot) moves with the upper leg during this orientation process. By default all joints are assigned stiffnesses, viscous characteristics, and stop angles which should give reasonable results in a crash simulation. One or all default values of a joint may be altered by applying the *COMPONENT_GEBOD_JOINT_OPTION command to the joint of interest. The default shape of the resistive torque load curve used by all joints is shown in Figure 57-6. A scale factor is applied to this curve to obtain the proper stiffness relationship. Listed in Table 57-3 are the default values of joint characteristics for dummies of all types and sizes. These values are given in the APPENDIX N English system of units; the appropriate units are used if a different system is specified in card 1 of *COMPONENT_GEBOD_OPTION. joint degrees of freedom load curve scale factor (in⋅lbf) damping coef. (in⋅lbf⋅s/rad) low stop angle (degrees) high stop angle (degrees) neutral angle (degrees) pelvis - 1 pelvis - 2 pelvis - 3 waist - 1 waist - 2 waist - 3 lower neck - 1 lower neck - 2 lower neck - 3 upper neck - 1 upper neck - 2 upper neck - 3 l. shoulder - 1 r. shoulder - 1 shoulder - 2 shoulder - 3 elbow - 1 l. hip - 1 r. hip - 1 hip - 2 hip - 3 knee - 1 l. ankle - 1 l. ankle - 1 ankle - 2 ankle - 3 65000 65000 65000 65000 65000 65000 10000 10000 10000 10000 10000 10000 100 100 100 100 100 10000 10000 10000 10000 100 100 100 100 100 5.77 5.77 5.77 5.77 5.77 5.77 5.77 5.77 5.77 5.77 5.77 5.77 5.77 5.77 5.77 5.77 5.77 5.77 5.77 5.77 5.77 5.77 5.77 5.77 5.77 5.77 -20 -20 -5 -20 -20 -35 -25 -25 -35 -25 -25 -35 -30 -175 -65 -175 1 -25 -70 -70 -140 -1 -30 -20 -20 -30 20 20 5 20 20 35 25 25 35 25 25 35 175 30 65 60 -140 70 25 70 40 120 20 30 45 30 Table 57-3. Default joint characteristics for all dummies. 0 0 0 0 0 0 0 0 0 0 0 0 0 0 0 0 0 0 0 0 0 0 0 0 0 APPENDIX N torque (-3.14,2.0) (-0.5,0.1) (0,0) (0.5,-0.1) rotation (radians) (3.14,-2.0) Figure 57-4 Characteristic torque curve shape used by all joints. The dummy depicted in Figure 57-1 appears in what is referred to as its "nominal" position. In this position the dummy is standing upright facing in the positive x direction and the toe-to-head direction points in positive z. Additionally, the dummy's hands are at the sides with palms facing inward and the centroid of the lower torso is positioned at the origin of the global coordinate system. Each of the dummy's segments has a local coordinate system attached to it and in the nominal position all of the local axes are aligned with the global axes. When performing a simulation involving a *COMPONENT_GEBOD dummy, a positioning file named "gebod.did" must reside in the directory with the LS-DYNA input file; here the extension did is the dummy ID number, see card 1 of *COMPO- NENT_GEBOD_OPTION. The contents of a typical positioning file is shown in Table 57-5; it consists of 40 lines formatted as (59a1,e30.0). All of the angular measures are input as degrees, while the lower torso global positions depend on the choice of units in card 1 of *COMPONENT_GEBOD_OPTION. Setting all of the values in this file to zero yields the so-called "nominal" position. Table 57-5. Typical contents of a dummy positioning file. lower torso lower torso lower torso total body total body total body centroid global x position centroid global y position centroid global z position global x rotation global y rotation global z rotation 0.0 0.0 0.0 0.0 -20.0 180.0 APPENDIX N pelvis pelvis pelvis waist waist waist lower neck lower neck lower neck upper neck upper neck upper neck left shoulder left shoulder left shoulder right shoulder right shoulder right shoulder left elbow right elbow left hip left hip left hip right hip right hip right hip left knee right knee left ankle left ankle left ankle right ankle right ankle right ankle lateral flexion forward flexion torsion lateral flexion forward flexion torsion lateral flexion forward flexion torsion lateral lexion forward flexion torsion abduction-adduction internal-external rotation flexion-extension abduction-adduction internal-external rotation flexion-extension flexion-extension flexion-extension abduction-adduction medial-lateral rotation flexion-extension abduction-adduction medial-lateral rotation flexion-extension flexion-extension flexion-extension inversion-eversion dorsi-plantar flexion medial-lateral rotation inversion-eversion dorsi-plantar flexion medial-lateral rotation + = tilt right + = lean fwd + = twist left + = tilt right + = lean fwd + = twist left + = tilt right + = nod fwd + = twist left + = tilt right + = nod fwd + = twist left + = abduction + = external - = fwd raise - = abduction - = external - = fwd raise + = extension + = extension + = abduction + = lateral + = extension - = abduction - = lateral + = extension + = flexion + = flexion + = eversion + = plantar + = lateral - = eversion + = plantar - = lateral 0.0 0.0 0.0 0.0 0.0 0.0 0.0 0.0 0.0 0.0 0.0 0.0 30.0 -10.0 -40.0 -30.0 10.0 -40.0 -60.0 -60.0 0.0 0.0 -80.0 0.0 0.0 -80.0 50.0 50.0 0.0 0.0 0.0 0.0 0.0 0.0 In Figure 57-6 the 50th percentile male dummy is shown in a seated position and some of its joints are labeled. The file listed in Table 57-5 was used to put the dummy into the position shown. Note that the dummy was first brought into general orientation by setting nonzero values for two of the lower torso local rotations. This is accomplished by performing right-handed rotations successively about local axes fixed in the lower torso, the sequence of which follows: the first about local x, next about local y, and the last about local z. The dummy in Figure 57-6 was made to pitch backward by setting APPENDIX N "total body global y rotation" equal to -20. Setting the "total body global z rotation" equal to 180 caused the dummy to rotate about the global z-axis and face in the -x direction. upper neck lower neck left elbow left shoulder waist pelvis left hip left knee left ankle Figure 57-6. Dummy seated using the file listed in Table 57-5. HYBRID III Dummies A listing of applicable joint degrees of freedom of the Hybrid III dummy is given below. APPENDIX N Joint Name lumbar lower neck upper neck 1st flexion (y) flexion (y) flexion (y) Degree(s) of Freedom 2nd torsion (z) torsion (z) torsion (z) shoulders flexion-extension (y) abduction-adduction (x) elbows flexion-extension (y) wrists flexion-extension (x) n/a n/a 3rd n/a n/a n/a hips abduction-adduction (x) medial-lateral rotation (z) flexion-extension (y) knees flexion-extension (y) n/a n/a ankles inversion-eversion (x) medial-lateral rotation (z) dorsi-plantar flexion (y) sternum translation (x) rotation (y) rotation (z) knee sliders translation (z) Table 57-7. Joints and associated degrees of freedom. Local axes are in parentheses. Joint springs of the *COMPONENT_HYBRIDIII dummies are formulated in the following manner. 𝑇 = 𝑎lo(𝑞 − 𝑞lo) + 𝑏lo(𝑞 − 𝑞lo)3, 𝑇 = 𝑎hi(𝑞 − 𝑞hi) + 𝑏hi(𝑞 − 𝑞hi)3, 𝑇 = 0, 𝑞 ≤ 𝑞lo 𝑞 ≥ 𝑞hi 𝑞lo < 𝑞 < 𝑞hi Where, T is the joint torque q is the joint generalized coordinate alo and blo are the linear and cubic coefficients, respectively, for the low regime ahi and bhi are the linear and cubic coefficients, respectively, for the high regime qlo and qhi are the activation values for the low and high regimes, respectively APPENDIX O APPENDIX O: LS-DYNA MPP User Guide This is a short user’s guide for the MPP version of LS-DYNA. For a general guide to the capabilities of LS-DYNA and a detailed description of the input, consult the LS-DYNA User's Manual. If you have questions about this guide, find errors or omissions in it, please email manual@lstc.com. SUPPORTED FEATURES The only input formats currently supported are 920 and later, including keyword input. Models in any of the older formats will need to be converted to one of these input formats before they can be run with the current version of LS-DYNA for massively parallel processors, mpp. The large majority of LS-DYNA options are available on MPP computers. Those that are not supported are being systematically added. Unless otherwise noted here, all the options of LS-DYNA version 93x are supported by MPP/LS-DYNA. Here is the list of unsupported features: *BOUNDARY_THERMAL_WELD *BOUNDARY_USA_SURFACE *CONTACT_1D *DATABASE_AVS *DATABASE_MOVIE *DATABASE_MPGS *LOAD_SUPERPLASTIC_OPTION *USER *TERMINATION_NODE CONTACT INTERFACES MPP/LS-DYNA uses a completely redesigned, highly parallel contact algorithm. The contact options currently unsupported include: Because these options are all supported via the new, parallel contact algorithms, slight differences in results may be observed as compared to the serial and SMP versions of LS-DYNA. Work has been done to minimize these differences, but they may still be evident in some models. For each of the supported CONTACT_control cards, there is an optional string_MPP which can be appended to the end. Adding these characters triggers the reading of a new control card immediately following (but after the TITLE card, if any). See the section on *CONTACT for details of the parameters and their meanings. OUTPUT FILES AND POST-PROCESSING For performance reasons, many of the ASCII output files normally created by LS-DYNA have been combined into a new binary format used by MPP/LS-DYNA. There is a post-processing program l2a, which reads this binary database of files and produces as output the corresponding ASCII files. The new binary files will be created in the directory specified as the global directory in the pfile . The files (up to one per processor) are named binoutnnnn, where nnnn is replaced by the four-digit processor number. To convert these files to ASCII simply feed them to the l2a program like this: l2a binout* LS-PREPOST is able to read the binout files directly, so conversion is not required, it is provided for backward compatibility. The supported ASCII files are: *DATABASE_SECFORC *DATABASE_RWFORC *DATABASE_NODOUT *DATABASE_NODOUTHF *DATABASE_ELOUT *DATABASE_GLSTAT *DATABASE_DEFORC *DATABASE_MATSUM *DATABASE_NCFORC *DATABASE_SPCFORC *DATABASE_SWFORC *DATABASE_DEFGEO *DATABASE_ABSTAT *DATABASE_NODOFR *DATABASE_BNDOUT *DATABASE_GCEOUT *DATABASE_RBDOUT *DATABASE_SLEOUT *DATABASE_JNTFORC *DATABASE_SBTOUT *DATABASE_SPHOUT *DATABASE_TPRINT Some of the normal LS-DYNA files will have corresponding collections of files produced by MPP/LS-DYNA, with one per processor. These include the d3dump files (new names = d3dump.nnnn), the messag files (now mesnnnn) and others. Most of these will be found in the local directory specified in the pfile. The format of the d3plot file has not been changed. It will be created in the global directory, and can be directly handled with your current graphics post-processor. PARALLEL SPECIFIC OPTIONS There are a few new command line options that are specific to the MPP version of LS- DYNA. In the serial and SMP versions of LS-DYNA, the amount of memory required to run the problem can be specified on the command line by adding “memory=XXX”, where XXX is the number of words of memory to be allocated. For the MPP code, this will result in each processor allocating XXX words of memory. If pre-decomposition has not been performed, one processor must perform the decomposition of the problem. This can require substantially more memory than will be required once execution has started. For this reason, there is a second memory command line option, “memory2=YYY”. If APPENDIX O used together with adding “memory=XXX”, the decomposing processor will allocate XXX words of memory, and all other processors will allocate YYY words of memory. For example, in order to run a 250,000 element crash problem on 4 processors, you might need memory=80m and memory2=20m. To run the same problem on 16 processors, you still need memory=80m, but can set memory2=6m. The value for memory2 drops nearly linearly with the number of processors used to run the program, which works well for shared-memory systems. Execution of the implicit solver in MPP requires a balance of memory across all of the processes. The user should not use memory2= specification for runs involving the implicit solver. If the model decomposition cannot be performed for the given memory= specification, one can try a pre-decomposition but the user would be advised to use a compute cluster with more real memory. It is suggested that the memory= specification be such to use no more than 75% of the real memory available to that process. On a compute cluster with each compute node having 48 Gbytes of memory and using 8 MPI processes, there is only 6 Gbytes of real memory per process. Converting to 8 byte words and using only the suggested 75% would have memory=560M as the maximum specification. The full deck restart capability is supported by the MPP version of LS-DYNA, but in a manner slightly different than the SMP code. Each time a restart dump file is written, a separate restart file is also written with the base name D3FULL. For example, when the third restart file d3dump03 is written (one for each processor, d3dump03.0000, d3dump03.0001, etc), there is also a single file written named d3full03. This file is required in order to do a full deck restart and the d3dump files are not used in this case by the MPP code. In order to perform a full deck restart with the MPP code, you first must prepare a full deck restart input file as for the serial/SMP version. Then, instead of giving the command line option r=d3dump03 you would use the special option n=d3full03. The presence of this command line option tells the MPP code that this is a restart, not a new problem, and that the file d3full03 contains the geometry and stress data carried over from the previous run. PFILE There is a new command line option: p = pfile. pfile contains MPP specific parameters that affect the execution of the program. The file is split into sections, with several options in each section. Currently, these sections: directory, decomposition, contact, and general are available. First, here is a sample pfile: directory { global rundir local /tmp/rundir } contact { APPENDIX O inititer 3 } The file is case insensitive and free format input. The sections and options currently supported are: directory: Holds directory specific options transfer_files If this option is given, then processor 0 will write all output and restart files to the global directory , and scratch files to the local directory. All other processors will write all data to their local directory. At normal termi- nation, all restart and output files will be copied from the processor specific local directories to the global directory. Also, if this is a restart from a dump file, the dump files will be distributed to the processors from the global directory. With this option enabled, there is no need for the processors to have shared access to a single disk for output – all files will be transferred as needed to and from the global directory. Default = disabled. global path Path to a directory where program output should be written. If transfer_files is not given, this directory needs to be accessible to all processors – otherwise it is only accessed by processor 0. This directory will be created if necessary. Default = current working directory global_message_files If this option appears, the message files are written in the global directory rather than the local directory Default = disabled (message files go in the local directory) local path Path to a processor specific local directory for scratch files. This directory will be created if necessary. This should be a local disk on each processor, for perfor- mance reasons. Default = global path rmlocal If this option is given and transfer_files is active, the program attempts to clean up the local directories on each processor. In particular, it deletes files that are successfully transferred back to the global directory, and removes the local directory if it was created. It will not delete any files if there is a failure during file copying, nor will it delete directories it did not create. Default = disabled repository path APPENDIX O Path to a safe directory accessible from processor 0. This directory will be creat- ed if necessary. This is intended to be used as a safekeeping/backup of files during execution and should only be used if transfer_files is also given. If this directory is specified then the following actions occur: • At program start up, any required files (d3dump, binout, etc) that can- not be located in the global directory are looked for in the repository for copying to the local processor directories. • Important output files (d3dump, runrsf, d3plot, binout and others) are synchronized to the repository regularly. That is, every time one of these files is updated on the node local or the global directories, a syn- chronized copy is updated in the repository. The intention is that the repository be on a redundant disk, such as NAS, to allow restarting the problem if a hardware failure should occur on the machine run- ning the problem. It must be noted that some performance penalty must be paid for the extra communication and I/O. Effort has been made to minimize this overhead, but this option is not recommended for general use. Default = unspecified decomposition: Holds decomposition specific options file filename The name of the file that holds the decomposition information. This file will be created in the current working directory if it does not exist. If this option is not specified, MPP/LS-DYNA will perform the decomposition. Default = None numproc n The problem will be decomposed for n processors. If n > 1 and you are running on 1 processor, or if the number of processors you are running on does not evenly divide n, then execution terminates immediately after decomposition. Otherwise, the decomposition file is written and execution continues. For a decomposition only run, both numproc and file should be specified. Default = the number of processors you are running on. method name Currently, there are two decomposition methods supported, namely rcb and greedy. Method rcb is Recursive Coordinate Bisection. Method greedy is a simple neighborhood expansion algorithm. The impact on overall runtime is problem dependent, but rcb generally gives the best performance. Default = rcb region rx ry rz sx sy sz c2r s2r 3vec mat See the section below on Special Decompositions for details about these decom- position options. APPENDIX O show If this option appears in the decomposition section, the d3plot file is doctored so that the decomposition can be viewed with the post processor. Displaying material 1 will show that portion of the problem assigned to processor 0, and so on. The problem will not actually be run, but the code will terminate once the initial d3plot state has been written. rcblog filename This option is ignored unless the decomposition method is RCB. A record is written to the indicated file recording the steps taken during decomposition. This is an ascii file giving each decomposition region and the location of each subdivision for that region. Except for the addition of this decomposition information, the file is otherwise equivalent to the current pfile. Thus it can be used directly as the pfile for a subsequent prob- lem, which will result in a decomposition as similar as possible between the two runs. For example, suppose a simulation is run twice, but the second time with a slightly different mesh. Because of the different meshes the problems will be distributed differently between the processors, resulting in slightly different answers due to roundoff errors. If an rcblog is used, then the resulting decompo- sitions would be as similar as possible. vspeed If this option is specified a brief measurement is taken of the performance of each processor by timing a short floating point calculation. The resulting information is used during the decomposition to distribute the problem according to the relative speed of the processors. This might be of some use if the cluster has machines of significantly different speed. automatic If this option is given, an attempt is made to automatically determine a reasona- ble decomposition, primarily based on the initial velocity of nodes in the model. Use of the show option is recommended to verify a reasonable decomposition. aledist Distribute ALE elements to all processors. dcmem n It may be in some cases that the memory requirements during the first phase of decomposition are too high. If that is found to be the case (if you get out of memory errors during decomposition phase 1), then this may provide a work around. Specifying a value n here will cause some routines to process the model in blocks of n items, when normal processing would read the whole set (of nodes, elements, whatever) all at once. This will reduce memory requirements at the cost of greater communication overhead. Most users will not need this option. Values in the range of 10,000 to 50,000 would be reasonable. APPENDIX O dunreflc Time dependent load curves are usually applied to the following boundary or loading conditions on each node. By default, those curves are copied to all MPP subdomain without checking for the presence of that node in the domain or not. The curves are evaluated every cycle and may consume substantial CPU time. This command will remove curves which are not referenced in the MPP subdo- main for the following keywords. *BOUNDARY_PRESCRIBED_MOTION_NODE *LOAD_NODE *LOAD_SHELL_ELEMENT *LOAD_THERMAL_VARIABLE_NODE timing_start n Begin timing of element calculations on cycle n. The appearance of this option will trigger the generation of a file named DECOMP_TIMINGS.OUT during normal termination. This file will contain information about the actual time spent doing element calculations, broken down by part. timing_end n End timing of element calculations on cycle n. A reasonable value is probably timing_start + 50 or 100. timing_file filename The file filename is assumed to be the output file DECOMP_TIMINGS.OUT from a previous run of this or a similar model. The computational cost of each part that appears in this file is then used during the decomposition instead of the built in internal value for that part. Matching is based strictly on the user part ID. The first two lines of the file are skipped, and only the first two entries on each of the remaining lines are relevant (the part ID and the cost per element). contact: This section has been largely replaced by the_MPP option on the normal contact card. The only remaining useful option here is: alebkt n Sets the bucket sort frequency for FSI (fluid structure interaction) to once every n cycles. default = 50 general: Holds general options APPENDIX O lstc_reduce If this option appears, LSTC’s own reduce routine is used to get consistent summation of floating point data among processors. See also, *CONTROL_MPP_- IO_LSTC_REDUCE which has the same effect.. nodump If this option appears, all restart dump file writing will be suppressed: d3dump, runrsf, and d3full files will not be written nofull If this option appears, writing of d3full (full deck restart) files will be suppressed. nod3dump If this option appears, writing of d3dump and runrsf files will be suppressed. runrsfonly If this option appears, writing of d3dump files will not occur – runrsf files will be witten instead. Any time a d3dump OR runrsf file would normally be written, a runrsf file will be written. nofail If this option appears, the check for failed elements in the contact routines will be skipped. This can improve efficiency if you do not have element failure in the model. swapbytes If this option appears, the d3plot and interface component analysis files are written in swapped byte ordering. nobeamout Generally, whenever a beam, shell, or solid element fails, and element failure report is written to the d3hsp and message files. This can generate a lot of out- put. If this option appears, the element failure report is suppressed. Special Decompositions: These options appear in the “decomposition” section of the pfile and are only valid if the decomposition method is rcb. The rcb decomposition method works by recursively dividing the model in half, each time slicing the current piece of the model perpendicularly to one of the three coordinate axes. It chooses the axis along which the current piece of the model is longest. The result is that it tends to generate cube shaped domains aligned along the coordinate axes. This is inherent in the algorithm, but is often not the behavior desired. APPENDIX O This situation is addressed by providing a set of coordinate transformation functions which are applied to the model before it is decomposed. The resulting deformed geometry is then passed to the decomposition algorithm, and the resulting domains are mapped back to the undeformed model. As a simple example, suppose you wanted rectangular domains aligned along a line in the xy plane, 30 degrees from the x axis, and twice as long along this line as in the other two dimensions. If you applied these transformations: sx 0.5 rz -30 then you would achieve the desired effect. Furthermore, it may be desirable for different portions of the model to be decomposed differently. It is now possible to specify different regions of the model to be decomposed with different transformations. The general form for a special decomposition would look like this: decomposition { region { <region specifiers> <transformation> <grouping> } region { <region specifiers> <transformation> <grouping> } <transformation> } Where the region specifiers are logical combinations of box, sphere, clinder, parts, and silist. The transformation is a series of sx, sy, sz, rx, ry, rz, c2r, s2r, 3vec, and mat. The grouping is either lumped or empty. The portion of the model falling in the first region will be decomposed according to the given transformation. Any remaining part of the model in the second region will then be treated, and finally anything left over will be decomposed according to the final transformation. Any number of regions may be given, including 0. Any number of transformations may be specified. They are applied to the region in the order given. The region specifiers are: box xmin xmax ymin ymax zmin zmax A box with the given extents. sphere xc yc zc r The sphere centered at (xc,yc,zc) and having radius r. If r is negative it is treated as infinite. cylinder xc yc zc ax ay az r d A cylinder with center at (xc,yc,zc) and radius r, extending out in the direction of (ax,ay,az) for a distance of d. If d is 0, the cylinder is infinte in both directions. APPENDIX O parts n1 n2 n3 n4…. All parts whose user id matches one of the given values are included in the region. Any number of values may be given. partsets n1 n2 n3 n4…. All partsets whose user id matches one of the given values will have all of their parts included in the region. Any number of values may be given. silist n1 n2 n3 n4…. All elements involved in a contact interface whose user id matches one of the given values are included in the region. The transformations available are: local This is only useful in conjunction with the *CONTROL_MPP_PFILE keyword option, when used inside a file included via *INCLUDE_TRANSFORM. At this point in the region processing, a transformation is inserted to invert the transfor- mation used by *INCLUDE_TRANSFORM. The effect is that if this option appears before any other transformation options, all those options (and the subsequent decomposition) are performed in the coordinate system of the include file itself, not the global coordinate system.. sx t scale the current x coordinates by t. sy t scale the current y coordinates by t. sz t scale the current z coordinates by t. rx t rotate around the current x axis by t degrees. ry t rotate around the current y axis by t degrees. rz t rotate around the current z axis by t degrees. txyz x y z translate by (x,y,z). mat m11 m12 m13 m21 m22 m23 m31 m32 m33 transform the coordinates by matrix multiplication: APPENDIX O Transformed Coordinates = 𝑥′ ⎤ = ⎡ 𝑦′ ⎥ ⎢ 𝑧′⎦ ⎣ 𝑚11 𝑚12 𝑚13 ⎥⎤ [ ⎢⎡ 𝑚21 𝑚22 𝑚23 𝑚31 𝑚32 𝑚33⎦ ⎣ ] 3vec v11 v12 v13 v21 v22 v23 v31 v32 v33 Transform the coordinates by the inverse of the transpose matrix: 𝑣11 ⎢⎡ 𝑣12 𝑣13 ⎣ 𝑣31 ⎥⎤ 𝑣32 𝑣33⎦ 𝑣21 𝑣22 𝑣23 𝑥′ ⎤ ⎡ 𝑦′ ⎥ ⎢ 𝑧′⎦ ⎣ ] = [ = VT × transformed coordinates This appears complicated, but in practice is very intuitive: instead of decomposing into cubes aligned along the coordinate axes, rcb will decompose into parallelipi- peds whose edges are aligned with the three vectors (v11, v12, v13), (v21, v22, v23), and (v31, v32, v33). Furthermore, the relative lengths of the edges of the decomposition domains will correspond to the relative lengths of these vectors. C2R x0 y0 z0 vx1 vy1 vz1 vx2 vy2 vz2 The part is converted into a cylindrical coordinate system with origin at (x0, y0, z0), cylinder axis (vx1, vy1, vz1) and theta = 0 along the vector (vx2, vy2, vz2). You can think of this as tearing the model along the (vx2, vy2, vz2) vector and unwrapping it around the (vx1, vy1, vz1) axis. The effect is to create decomposi- tion domains that are “cubes” in cylindrical coordinates: they are portions of cylindrical shells. The actual transformation is: new(𝑥, 𝑦, 𝑧) = cylindrical coordinates(𝑟, 𝜃, 𝑧) Knowing the order of the coordinates is important if combining transformations, as in the example below. S2R x0 y0 z0 vx1 vy1 vz1 vx2 vy2 vz2 Just like the above, but for spherical coordinates. The (vx1,vy1,vz1) vector is the phi = 0 axis. new(𝑥, 𝑦, 𝑧) = spherical coordinates(𝜌, 𝜃, 𝜙) The grouping qualifier is: lumped Group all elements in the region on a single processor. If this qualifier is not given, the elements in the region are distributed across all processors. Examples: rz 45 will generate domains rotated -45 degrees around the z axis. APPENDIX O C2R 0 0 0 0 0 1 1 0 0 will generate cylindrical shells of domains. They will have their axis along the vector (0,0,1), and will start at the vector (1,0,0) Note that the part will be cut at (1,0,0), so no domains will cross this boundary. If there is a natural boundary or opening in your part, the “theta = 0” vector should point through this opening. Note also that if the part is, say, a cylinder 100 units tall and 50 units in radius, after the C2R transformation the part will fit inside the box x=[0,50], y=[0, 2PI), z=[0,100]. In particular, the new y coordinates (theta) will be very small com- pared to the other coordinate directions. It is therefore likely that every decom- position domain will extend through the complete transformed y direction. This means that each domain will be a shell completely around the original cylinder. If you want to split the domains along radial lines, try this pair of transfor- mations: C2R 0 0 0 0 0 1 1 0 0 SY 5000 This will do the above C2R, but then scale y by 5000. This will result in the part appearing to be about 30,000 long in the y direction -- long enough that every decomposition domain will divide the part in this (transformed) y direction. The result will be decomposition domains that are radial “wedges” in the origi- nal part. General combinations of transformations can be specified, and they are applied in order: SX 5 SY .2 RZ 30 will scale x, then y, then rotate. A more general decomposition might look like: decomposition { rx 45 sz 10 region { parts 1 2 3 4 5 and sphere 0 0 0 200 lumped } region { box 0 100 –1.e+8 1.e+8 0 500 or sphere 100 0 200 200 rx 20 } } This would take elements that have user ID 1, 2, 3, 4, or 5 for their part, AND that lie in the sphere of radius 200 centered at (0,0,0), and place them all on one processor. Then, any remaining elements that lie in the given box OR the sphere of radius 200 centered at (100,0,200) would be rotated 20 degress in x then decomposed across all processors. Finally, anything remaining would be rotated 45 degrees in x, scaled 10 in z, and distributed to all processors. In general, region qualifiers can be combined using the logical operations and, or, and not. Grouping using parentheses is also supported. APPENDIX O EXECUTION OF MPP/LS-DYNA MPP/LS-DYNA runs under a parallel environment which provided by the hardware vendor. The execution of the program therefore varies from machine to machine. On some platforms, command line parameters can be passed directly on the command line. For others, the use of the names file is required. The names file is supported on all systems. The serial/SMP code supports the use of the SIGINT signal (usually Ctrl-C) to interrupt the execution and prompt for user input, generally referred to as “sense switches.” The MPP code also supports this capability. However, on many systems a shell script or front end program (generally “mpirun”) is required to start MPI applications. Pressing Ctrl-C on some systems will kill this process, and thus kill the running MPP-DYNA executable. As a workaround, when the MPP code begins execution it creates a file “bg_switch” in the current working directory. This file contains the following single line: rsh <machine name> kill -INT <PID> where < machine name > is the hostname of the machine on which the root MPP-DYNA process is running, and <PID> is its process id. (on HP systems, “rsh” is replaced by “remsh”). Thus, simply executing this file will send the appropriate signal. Here is a simple table to show how to run the program on various platforms. Of course, scripts are often written to mask these differences. Platform Execution Command DEC Alpha dmpirun –np n mpp-dyna Fujitsu Hitachi HP IBM NEC SGI Sun jobexec –vp n –mem m mpp-dyna mpirun –np n mpp-dyna mpp-dyna –np n #!/bin./ksh export MP_PROC=n export MP_LABELIO=no export MP_EUILIB=us export MPI_EUIDEVICE=css0 poe mpp-dyna mpirun –np n mpp-dyna mpirun –np n mpp-dyna tmrun –np n mpp-dyna Where n is the number of processors, mpp-dyna is the name of the MPP/LS-DYNA executable, and m is the MB of real memory. APPENDIX O APPENDIX P APPENDIX P: Implicit Solver INTRODUCTION The terms implicit and explicit refer to time integration algorithms. In the explicit approach, internal and external forces are summed at each node point, and a nodal acceleration is computed by dividing by nodal mass. The solution is advanced by integrating this acceleration in time. The maximum time step size is limited by the Courant condition, producing an algorithm which typically requires many relatively inexpensive time steps. While explicit analysis is well suited to dynamic simulations such as impact and crash, it can become prohibitively expensive to conduct long duration or static analyses. Static problems such as sheet metal springback after forming are one application area for implicit methods. In the implicit method, a global stiffness matrix is computed, inverted, and applied to the nodal out-of-balance force to obtain a displacement increment. The advantage of this approach is that time step size may be selected by the user. The disadvantage is the large numerical effort required to form, store, and factorize the stiffness matrix. Implicit simulations therefore typically involve a relatively small number of expensive time steps. In a dynamic implicit simulation these steps are termed time steps, and in a static simulation they are load steps. Multiple steps are used to divide the nonlinear behavior into manageable pieces, to obtain results at intermediate stages during the simulation, or perhaps to resolve a particular frequency of motion in dynamic simulations. In each step, an equilibrium geometry is sought which balances dynamic, internal and external forces in the model. The nonlinear equation solver performs an iterative search using one of several Newton based methods. Convergence of this iterative process is obtained when norms of displacement and/or energy fall below user-prescribed tolerances. Within each implicit iteration there is a line search performed for enhancing robustness of the procedure. The implicit analysis capability was first released in Version 950. Initially targeted at metal forming springback simulation, this new capability allowed static stress analysis. Version 970 added many additional implicit features, including new element formulations for linear and modal analysis. A milestone in implicit was the advent of Version 971 in which implicit analysis was carried over to MPP and thus allowed much larger problems to be solved, and from there it has evolved extensively to presently contend well among competitive softwares. Still, it can be a gruesome task to set up an implicit input problem that runs all the way to completion with acceptable results, especially when contacts are involved. The purpose of this text is to explain keywords of interest and suggest values of important parameters in order to give users tools for developing own solution strategies to these kinds of problems. APPENDIX P A prerequisite for running implicit is to use a double precision version of LS-DYNA, and a machine with a significant amount of memory. A theoretical overview of implicit can be found in the LS-DYNA Theory Manual implicittheorychapter. NONLINEAR IMPLICIT ANALYSIS Activating Implicit Analysis The keyword *CONTROL_IMPLICIT_GENERAL is used to activate the implicit method, and in principle it is sufficient to set IMFLAG = 1 DT0 = some reasonable initial time step. The initial time step should be chosen small enough to resolve the frequency spectrum of interest and/or provide decent convergence properties, but large enough to benefit from an implicit analysis. With no other implicit options, this converts an explicit input deck to a static implicit input deck with a constant time step throughout the simulation and the problem will terminate upon convergence failure. Time stepping strategies to prevent this are discussed Time Stepping Strategies Singularities and Eigenvalue Analysis The first concern in implicit analysis is to prevent singularities in the stiffness matrix, otherwise the chance of succeeding is close to none. The major source to a singular stiffness matrix is the presence of rigid body modes in a static problem, and these can be revealed using *CONTROL_IMPLICIT_EIGENVALUE and putting eigenvalue analysis. done This by an in is NEIG = number of modes to extract. Run an eigenvalue analysis and extract (if practically possible) enough modes to see all the rigid body modes just to get an impression of the properties of the model. The frequencies are in the output text file “eigout” and the mode shapes can be animated in the binary output file “d3eigv” using LS-PrePost. Some rigid body modes may come as a surprise and should be constrained, a typical example of this are beams that are free to rotate around its own axis. Other rigid body modes are a consequence of the nature of the problem and cannot be constrained without destroying the connection to reality, an example of this could be components that are to be constrained with contacts but are initially free to move. There are several strategies to deal with these latter rigid body modes, some are discussed in the context of contacts but here dynamics is used. Dynamics and Intermittent Eigenvalue Analysis Dynamics *CONTROL_IMPLICIT_DYNAMICS by putting alleviates singular rigid body modes and is activated on APPENDIX P IMASS = 1 or a negative number. If the purpose is to solve a dynamic problem in the first place, then just use IMASS = 1 and don’t bother about the other parameters, otherwise some other strategy is necessary. The idea is to get off to a start using dynamic analysis, and as the simulation gets to a point where rigid modes have been constrained by contacts, dynamics is turned off. The simplest way of doing this is to put TDYBIR = 0 TDYDTH = time when contacts have been established and rigid body modes are constrained TDYBUR = time after TDYDTH for fading out dynamics between TDYDTH and TDYBUR. If the dynamic results are of no interest but just a way to proceed to the static solution, then it is recommended to use numerical damping to prevent unnecessary oscillations, i.e., put GAMMA = 0.6 BETA = 0.38. This should be enough to start up most problems of interest. A restriction with this is that when dynamics has been turned off it cannot be turned on again. If this is necessary for some reason, then a negative number of IMASS should be used to control dynamics through a load curve. If it is hard to deduce how to choose the time when to turn off dynamics, the use of intermittent eigenvalues may be of great help. By putting NEIG = a negative number on *CONTROL_IMPLICIT_EIGENVALUE the user may extract eigenvalues at given time points during a nonlinear simulation and deduce from that if all rigid body modes have been eliminated. The Geometric Stiffness Contribution Stiffness singularities may also occur during simulation due to a complex global phenomenon involving the stress state and geometry. For instance could slender components with compressive stresses give rise to zero eigenvalues, commonly known as buckling. The mathematical explanation to these kinds of singularities is that the material and geometric stiffness contributions cancel out, and for this reason the geometric contribution to the stiffness matrix is in LS-DYNA optional. It is activated by putting APPENDIX P IGS = 1 on *CONTROL_IMPLICIT_GENERAL. this contribution have a negative effect on convergence although it sometimes helps. It is recommended to leave this as default and turn it on if other strategies fail. A controlled way of getting past singular points of this type is to use so called arc length methods for which the geometric stiffness should be turned on, this way of dealing with the problem is discussed in the Theory Manual arclengthchapter. Most often singularities due to BFGS or Full Newton The nonlinear solver parameters are set on *CONTROL_IMPLICIT_SOLUTION where the solver type is specified as NSOLVR = nonlinear or linear implicit analysis option By default, a nonlinear BFGS solution strategy is used where the stiffness matrix is reformed every 11th iteration and a maximum of 15 reformations is allowed (for a linear solution set NSOLVR = 1). These parameters are set by ILIMIT = iterations between reforming stiffness matrix MAXREF = maximum number of stiffness reformations on *CONTROL_IMPLICIT_SOLUTION. Reforming the stiffness matrix is computa- tionally expensive but stabilizes the solution procedure, and the best strategy in this context is very much problem dependent. The recommendation is to start with the default strategy and if necessary change them. For hard problems decrease ILIMIT and for problems that converge well increase ILIMIT. For really bad problems switch to full Newton (the safe bet) by for instance putting ILIMIT = 1 MAXREF = 30. Keep the maximum number of reformations reasonably low or otherwise it may take an unnecessary amount of time just to reach convergence failure. Convergence Tolerances Convergence is based on changes in displacements, energies and optionally residual forces, and the tolerance levels are set by DCTOL = Relative displacement tolerance ment tolerance ECTOL = Relative energy tolerance tolerance DMTOL = Maximum displace- EMTOL = Maximum energy APPENDIX P RCTOL = Relative residual tolerance ABSTOL = Absolute tolerance RMTOL = Maximum residual tolerance on *CONTROL_IMPLICIT_SOLUTION. The tolerances on the left are based on Euclidian norms of the involved vectors, whereas the ones on the right are based on maximum norms. The maximum norm tolerances are optional and should be activated if increased accuracy is desired at the price of more implicit iterations. To keep things simple, the discussion that follows pertains only to the Euclidian norm tolerances. By default, the progress of the equilibrium search is not shown to the screen but can be activated using NLPRINT = nonlinear output diagnostics input parameter. The box below shows a typical iteration sequence, where the norms of displacement and energy are displayed. When these norms are reduced below user prescribed tolerances (default 0.001 and 0.01, respectively), the iteration process is said to have converged, and the solution proceeds to the next time step. The message files, messag in SMP and mesXXXX in MPP, typically contain a whole lot more information that will be dealt with further in Output and Stretching for Convergence. BEGIN static time step 3 ============================================================ time = 1.50000E-01 current step size = 5.00000E-02 Iteration: 1 *|du|/|u| = 3.4483847E-01 *Ei/E0 = 1.0000000E+00 Iteration: 2 *|du|/|u| = 1.7706435E-01 *Ei/E0 = 2.9395439E-01 Iteration: 3 *|du|/|u| = 1.6631174E-03 *Ei/E0 = 3.7030904E-02 Iteration: 4 *|du|/|u| = 9.7088516E-05 *Ei/E0 = 9.6749731E-08 Premature Convergence The last of these parameters (ABSTOL) overrides the other three (DCTOL, ECTOL, RCTOL) in the sense that if the residual force is small enough, convergence is detected regardless if the other three criteria are fulfilled or not. It has been seen that this sometimes give rise to so called premature convergence, converged states are not really converged in the sense that the residual norm is small enough. This gives bad results and it is usually recommended to tighten this tolerance to 10−20 to prevent this. On the other hand, if the problem is very hard this may prevent convergence to the extent that going back to the default is more or less necessary. It is difficult to give a general recommendation that holds for every problem. As for the other three parameters, the one that usually comes into practice is the displacement criterion DCTOL. The energy criterion ECTOL is often easy to fulfill and the residual criterion is disabled by default and there may be no reason to activate this (that is unless a completely Using Residual Tolerance is used, or if Stretching for Convergence arise). Using the default values on all three is usually good enough to give acceptable results in decent time. For problems with poor convergence, the question of tightening or relaxing these parameters (that is the displacement APPENDIX P convergence criterion) is up for debate. It is tempting to believe that relaxing the constraints will give better convergence which may or may not be true. Sloppy convergence criteria may once again result in premature convergence, and this will have a negative effect on the subsequent steps. The general recommendation would have to be to leave these unchanged, and be aware that relaxing them may not result in getting further in the implicit simulation. Using Residual Tolerance A novel strategy that seems to make sense and works well for some problems is to only use tolerances on residual forces RCTOL. This relies much on that the degree of nonlinearity of the simulation model is moderate, but it could be well worth trying. The first thing to do would be to put DCTOL and ECTOL to large numbers to disable them and put RCTOL to a relatively small number, start with 0.01 and see how that works out. This must be complemented with an absolute tolerance on the residual forces to get past the initial stages where the residual forces are small enough to not fulfill the relative tolerance. This is done by putting ABSTOL to a negative number, which is a different absolute criterion compared to putting it to a positive number. Now, this number is very problem dependent as this says that convergence is attained as soon as the Euclidian norm of the residual force vector is smaller than the absolute value of ABSTOL. It goes without saying that this require running the problem for a few steps to monitor the residual norm in the message files as described below, this should give an indication on how to determine the ABSTOL value. Convergence Norms The degrees of freedom encountered in an LS-DYNA simulation are either translational or rotational, where the latter comes from the presence of beams and shells. Historically, convergence check is on norms of the translational degrees of freedom only, which is unsettling from the fact that rotational residual forces (moments) are equally important in an implicit simulation. It is therefore recommended to use NLNORM = choice of convergence norms on *CONTROL_IMPLICIT_SOLUTION to change this default (which is = 2). While NLNORM = 3 will incorporate residual degrees of freedom separately and is a more satisfying approach, the recommended option is to use NLNORM = 4 or NLNORM a negative number. NLNORM = 4 will treat the entire force and displacement vector, respectively, as one complete mathematical vector and the convergence norms and scalar products used for checks are simply the Euclidian norms of these vectors. This will make the energy norm unit consistent since each term in the scalar product is an energy quantity, either through force times displacement or moment times angular increment. The displacement norm and residual norm, however, contains a mix of translational and rotational quantities which means that displacements are summed to angular increments and forces are summed to moments. This is of course not pretty, but it can be interpreted as using a length scale of 1 for the rotational degrees of freedom, meaning that displacements are summed to 1 length unit times angular APPENDIX P increments, and moments are summed to 1 length unit times forces. If the model is in length units of 𝑚𝑚, and the element sizes are in the order of 1 𝑚𝑚, this seems to be a reasonable length scale. But if the length unit is something else, it is convenient to use NLNORM = -(length scale) to scale with the number that corresponds to 1 𝑚𝑚. If for instance the length unit is 𝑚, then NLNORM = -0.001 is presumably a reasonable choice. Time Stepping Strategies By default, LS-DYNA will terminate when a step fails to converge. This is unfortunate since it may just be that the step is too large to achieve convergence and taking smaller steps would solve this problem. Instead of starting all over with a smaller step size, set IAUTO = 1 to activate automatic time stepping on *CONTROL_IMPLICIT_AUTO. When the problem fails to converge LS-DYNA will with this option go back to the previously converged state and retry with a smaller step size. If the problem converges well, the step size is increased for subsequent steps. This process of backing up and retrying difficult steps lends much persistence to the analysis, and is often the only procedure for solving highly nonlinear problems short of adjusting the step size manually and the recommendation is to always turn automatic time stepping on. Another parameter worth mentioning in this context is DTMAX = Max time step allowed, or a negative number on the same card. This is the maximum step size possible and should be chosen so as to not loose necessary information in the results, i.e., be sure to resolve frequencies, contacts and nonlinear material response to a satisfactory degree. A negative value of this parameter will give the maximum step size as a function of the simulation time and also allows for hitting key points that are of interest. The user may for instance look for the peak stress for a certain external load and hitting the point in time when this happens is crucial. It also allows for taking smaller steps during critical stages in the simulation without wasting resources away from these stages. Line Search A good line search strategy is crucial in solving nonlinear implicit problems, without it only simple problems would be solvable. There are a few line search options available and these are activated by LSMTD = Line search method on *CONTROL_IMPLICIT_SOLUTION. The default method is based on minimizing a potential energy along the search direction and at the same time keeping track of the residual force magnitude. It also detects when a BFGS step results in negative initial energy and the stiffness matrix is reformed for robustness (this can only happen when APPENDIX P the stiffness matrix has negative eigenvalues), and even suppresses the occurrence of negative volumes. Line search type 2 is based on residual forces and is more robust than the others, the drawback is that it typically results in too small steps and is not practically useful. Line search type 3 is very similar to type 4, but is not tracking the residual force or avoids negative volumes to the same extent, and in sum there is no practical reason for choosing methods 1 through 3. Worth mentioning is however line search type 5 which combines the energy and residual method in a stricter sense. That is, it minimizes the potential energy just like type 4 but it only allows the residual norm to double at each implicit iteration. This has shown to be robust but on the other hand slow in convergence and is to be used for problems that have difficulties to converge with the default line search strategy. This has had a huge impact on the treatment of rubber models for instance. An interesting combination is to use line search method 5 together with the strategy of converging based onUsing Residual Tolerance. Finally, the line search tolerance LSTOL = Line search tolerance on *CONTROL_IMPLICIT_SOLUTION is fine as it is, don’t change it. Output As previously mentioned, the output to the message file is more extensive than that to the screen/stdout. To novice or average implicit users this information may be more than can be digested at first and this section may be LINEAR EQUATION SOLVER, but with experience the output can become really useful when running into convergence issues. For this discussion it is important to distinguish between different types of iterations, and we use the term time/load step to mean the actual advance in simulation time, implicit iteration to indicate points in the iterative solution procedure where a new search direction is obtained (corresponding to either Newton or BFGS) and line search iteration to indicate the search for an optimal step size along a given search direction. We begin by showing a typical iteration output for when NLPRINT = 3 following by a bulletin list explaining the content. 1BEGIN implicit dynamics step 2 t = 2.5849E-01 ============================================================ time = 2.58489E-01 current step size = 1.58489E-01 . . . 2Newton step computed Initial translational energy = 1.4031740E-01 3Initial total energy = 1.4031740E-01 Initial residual norm = 7.5755334E-01 4Translational nodes norm = 7.1314670E-01 Translational nodes max = 1.9159278E-01 at node 440788 Translational rigid body norm = 3.5324028E-03 Translational rigid body max = 2.3897586E-03 at body 4000024 APPENDIX P Rotational rigid body norm = 2.5553155E-01 Rotational rigid body max = 1.7834357E-01 at body 4000024 5Evaluated residual for full step Current translational energy = 9.0141343E-02 6Current total energy = 9.0141343E-02 Current residual norm = 2.2038666E+00 Translational nodes norm = 2.1950775E+00 Translational nodes max = 1.0295509E+00 at node 440984 Translational rigid body norm = 3.4677960E-02 Translational rigid body max = 2.6701145E-02 at body 4000024 Rotational rigid body norm = 1.9354585E-01 Rotational rigid body max = 1.2669458E-01 at body 4000024 7Evaluated residual for step size 6.6666667E-01 Current translational energy = 1.1123844E-01 Current total energy = 1.1123844E-01 Current residual norm = 1.5007375E+00 Translational nodes norm = 1.4922142E+00 Translational nodes max = 7.1187918E-01 at node 440984 Translational rigid body norm = 1.6121536E-02 Translational rigid body max = 1.2659274E-02 at body 4000024 Rotational rigid body norm = 1.5890244E-01 Rotational rigid body max = 1.0852930E-01 at body 4000024 Evaluated residual for step size 3.3333333E-01 Current translational energy = 1.2543971E-01 Current total energy = 1.2543971E-01 Current residual norm = 8.3754668E-01 Translational nodes norm = 8.1775945E-01 Translational nodes max = 3.0290699E-01 at node 440984 Translational rigid body norm = 5.4770134E-03 Translational rigid body max = 4.5377150E-03 at body 4000024 Rotational rigid body norm = 1.8089755E-01 Rotational rigid body max = 1.2913973E-01 at body 4000024 Line search continues Max relative step = 0.3499001E+00 8Lower bound = 3.3333333E-01 Upper bound = 1.0000000E+00 Evaluated residual for step size 7.7777778E-01 Current translational energy = 1.0487486E-01 Current total energy = 1.0487486E-01 Current residual norm = 1.7421066E+00 Translational nodes norm = 1.7342352E+00 Translational nodes max = 8.2830775E-01 at node 440984 Translational rigid body norm = 2.1464316E-02 Translational rigid body max = 1.6693623E-02 at body 4000024 Rotational rigid body norm = 1.6402030E-01 Rotational rigid body max = 1.0799892E-01 at body 4000024 Evaluated residual for step size 5.5555556E-01 Current translational energy = 1.1674955E-01 Current total energy = 1.1674955E-01 Current residual norm = 1.2575584E+00 Translational nodes norm = 1.2472759E+00 Translational nodes max = 5.8455890E-01 at node 440984 Translational rigid body norm = 1.1655353E-02 Translational rigid body max = 9.2884622E-03 at body 4000024 APPENDIX P Rotational rigid body norm = 1.6006264E-01 Rotational rigid body max = 1.1222751E-01 at body 4000024 9Line search converged in 2 iterations 10Max relative step = 7.1106671E-01 11Iteration: 5 displacement energy residual ---------- not conv. not conv. converged norm ratio 1.013E+00 1.000E+00 n/a current norm 8.446E-01 1.403E-01 1.258E+00 initial norm 8.338E-01 1.403E-01 7.575E+00 ------------- trans rot trans rot trans rot max node norm 8.533E-02 0.000E+00 2.052E-02 0.000E+00 5.846E-01 0.000E+00 at node ID 4000674 9007526 440984 9007526 440984 9007526 ------------- RB max 3.449E-02 6.613E-04 -5.507E-04 7.681E-05 9.288E-03 1.122E- 01 at RB ID 4000024 4000024 4000024 4000024 4000024 4000024 Referring to the superscripts at the beginning of the lines in the excerpt above, and taking them in order of appearance, we have at 1.Beginning a dynamic implicit time/load step, the goal is to get to a given time point (in this case 2.5849E-01 using a step size of 1.58489E-01). Implicit time/load steps are either dynamic, static or semidnmc, where the last one indicates a transi- tion phase between dynamics and statics. 2.A Newton implicit iteration is performed, meaning that a full reformation of the stiffness matrix has just been made. Other implicit iterations can be either a linear if at the first iteration of a time/load step, or BFGS if the implicit iteration corresponds to a quasi-Newton step. 3.Initial norms are displayed at the beginning of each implicit iteration, these numbers are used as reference for the line search algorithm when checking line search convergence. 4.Detailed initial norms are displayed, separating out translational/rotational as well as nodal/rigid body Euclidian/max norms. The node number and rigid body attaining the global maximum norms are displayed and can be used to spot critical points in the model, in this particular case node 440984 and part 4000024 would be the likely candidates to trouble. 5.A full step along the search direction is taken, as a candidate for the next implicit iteration. 6.Norms for the full step is displayed, the line search algorithm compares these with the ones from 3 to deduce if line search convergence criterion is fulfilled. 7.Line search is in this case needed, and information for further iterates along the search direction is displayed in analogy to previous line search iterates. If no line search had been needed, the string Line search is skipped would have been dis- played. 8.The way line search is performed, each line search iteration narrows in on the optimal step and the bounds within which the optimal step is sought is continu- ously displayed. The size of this interval becomes smaller and smaller with APPENDIX P increasing number of line search iterations, but convergence should preferably be attained before it tends to zero. 9.Line search converged here in 2 iterations; as a rule of thumb the number of iterations for line search should be about 10 or less. For critical steps one might accept 20 iterations but that should be among the exceptions. If the string Line search did not converge is displayed, that is an indication of something being terribly wrong. 10.After each implicit iteration, Max relative step indicates how large steps have been taken during line search so far. It also indicates how well prescribed motion is approximated where a value of 1 is perfect. For values below 1 and in the pres- ence of non-zero prescribed motion, convergence will not be accepted even though all norms are within prescribed tolerances. This will instead issue the warning Convergence prevented due to unfulfilled boundary conditions and iterations continue. 11.Diagnostics for iteration 5 is displayed, similar numbers as shown during line search but in another format. Furthermore, the initial norms here refer to the initial norms from the beginning of the implicit time/load step and not from the beginning of the implicit iteration. This table can be used to deduce how close the implicit time/load step is at converging. The single important number for comfortably assessing the accuracy of an implicit iterate is the residual norm, currently displayed as 1.258E+00 (bold-faced in the table), since this should be small for good results. At equilibrium, the output ends with a summary on how convergence was achieved. It may look like Convergence detected as a combination of 1.Ratio of euclidian displacement Value = 2.3417E-03 vs Tolerance = 2.5000E-3 2.Ratio of euclidian energy Value = 3.2269E-08 vs Tolerance = 1.0000E-2 which tells us that the ratio of displacement was below DCTOL = 2.5E-3 and the ratio of energy was below ECTOL = 1E-2. If other criteria are satisfied, these will be listed too. So, with NLPRINT = 3 information from every force evaluation is given, including type of step taken, the line search step size, the potential energy value used in line search and the magnitude of the residual force. A point is made here, already Premature Convergence and will be repeated, and it is the following. The nonlinear implicit solver is solving for zero residual force, so basically the number observed for the magnitude of the residual force should be small upon convergence (bold-faced in the table). If it is not, then the convergence is premature and the results may not be correct and subsequent steps are in danger. What “small” means in this context is hard to say since this depends on units as well as loads and geometry of the problem, but a good sign is that the residual force does not grow by more than the external loads in the problem do. Another thing to observe is how the Line Search is doing, if the line search starts APPENDIX P needing many iterations and very large variations in the residual force along the search direction is observed, then it is likely that something in the model is causing this behavior. A safe bet is that contact states are changed along the line search direction causing discontinuities in the residual force and indicates that some remodeling has to be done. We will come back to this section when discussion Taking Advantage of ASCII Information and strategies to prevent them. LINEAR EQUATION SOLVER General Within each equilibrium iteration, a linear system of equations of the form 𝑲𝛥𝒖 = 𝑹 must be solved. To do this, the stiffness matrix 𝑲 is factorized and applied to the out- of-balance load or residual 𝑹, yielding a displacement increment 𝛥𝒖. Storing and solving this linear system represents a large portion of the memory and CPU costs of an implicit analysis. LS-DYNA uses a multi-frontal sparse direct solver and nested dissection, and for a problem with 𝑁 number of nodes, the number of operations and memory storage is asymptotically proportional to 𝑁3/2 and 𝑁𝑙𝑜𝑔𝑁, respectively. This should give a ballpark indication on the growth when increasing the size of a given model. It must be stressed however that it is a priori difficult to predict the actual value of these numbers as they are highly dependent on the problem solved, in particular on the nodal connectivity through elements and contacts. In the end we are left at qualitative guessing how to set memory flags or determining model size in order to push the limits for a given computer architecture. We here focus on the memory, and the purpose is twofold. First it is a documentation of the memory diagnostics that is written to the output message files (messag in SMP and mesXXXX in MPP) of LS-DYNA for the linear solvers. The level of information is regulated by the LPRINT = Linear solver diagnostics level input parameter on *CONTROL_IMPLICIT_SOLVER, and this text will cover LPRINT = 2 as the information for higher values is of no particular interest to others than developers. Second it should help understanding the interrelationship between the size of a model and the memory required to obtain a solution. We emphasize however that different classes of problems most likely require different guidelines (shell and solid structures typically result in different matrix topologies for instance) and to this end the user is left at earning this experience on his own. Memory The memory is specified and reported in terms of words, where 1 word is equivalent to 4 bytes in single precision and 8 bytes in double precision arithmetic. To simplify things, APPENDIX P a word can in this context be seen as the equivalent of a real number or an integer. For implicit calculations the executable used is typically double precision, so to convert from words to bytes one needs to multiply by 8. In starting a simulation the user typically specifies the static memory, for instance in SMP ls-dyna i = in.k memory = 200m meaning that LS-DYNA tries to allocate 200 Mwords for storing most of the data. In MPP, the physical memory is distributed among processes and this option applies to each individual process. In MPP there is also an option to add a second memory flag, for instance mpp-dyna i = in.k memory = 1000m memory2 = 200m and this means that 200 Mwords are allocated for each process while 1000 Mwords is allocated on the first process to handle everything up to the point when the model data has been distributed among all the involved processes. The memory size may also be specified on *KEYWORD. For implicit it is recommended to avoid memory2 in order to keep the memory balance between processors. When a certain feature requires a slot in the memory, this is reported in the output text files, for instance as contracting memory to 2306940 implicit friction expanding memory to 2306955 joints In the example above, the memory pointer after having allocated for implicit friction is at 2306940 and joints reserves 15 words and increment the memory pointer accordingly. So the memory used up to this point is roughly 2.3 Mwords for this particular process. At the end of the initialization a memory report is written and can look like S t o r a g e a l l o c a t i o n Memory required to begin solution : 2680153 Linear Alg dynamically allocated memory: 880685 Additional dynamically allocated memory: 1553130 Total: 5113968 The total amount of memory used up to this point is roughly 5.1 Mwords, which is partitioned in the static memory specified and dynamic memory that is allocated on the fly so to speak, typically if a certain amount of memory needed cannot be estimated in due time to adequately include it in the static chunk of memory. Whenever a memory violation occurs, for instance when trying to allocate more memory than physically available or if more memory needs to be specified, LS-DYNA terminates with appropriate error information. The static memory for the linear solver is allocated thereafter, which is the topic for the next section. APPENDIX P Linear Solver Memory Consumption For LPRINT = 2, some memory information is given in the output files, and this is here presented in order of execution, thus as they appear in the files. We repeat that this is the information obtained in the message files and is thus referring to the memory consumption for this particular process if MPP is considered. For the sake of completeness we also cover the diagnostics related to the CPU time for the involved stages in the linear solution. First the memory required for handling constraints is reserved and is reported as expanding memory to 2893375 implicit lsolvr allocation 1 After this memory is reserved for symbolic factorization, which is performed prior to the actual solve to predict the storage requirement for the factorized system matrix. This allocation is reported as expanding memory to 7639758 implicit matrix storage Also, some memory is reserved for the sparse matrix, including index pointers to non- zero elements, and is reported as expanding memory to 15077248 linear eqn. solver allocation 2d Here the last information (2d) is referring to the solver used and may change depending on user options. Before the symbolic factorization takes place, current information on the system matrix and workspace reserved for implicit is reported local number of rows = 68490 local size of matrix = 2338945 local len of workspace = 15077248 ptr to start of wrkspc = 2893375 The first number refers to the number of independent degrees of freedom in the model, i.e., the number of rows in the system matrix, and the second to the number of nonzero entries before factorization takes place, i.e., after assembly. The third row of information is somewhat misleading as this is actually the total amount of memory reserved and not the size of the workspace itself. The workspace here means the memory reserved for the linear solution, and its size is obtained by subtracting the pointer to start of workspace and the local length of workspace. The symbolic factorization is now performed and information on the CPU time for doing this together with the estimated size of the factorized matrix is reported CPU: symbolic factor = 0.200 WCT: symbolic factor = 0.203 storage currently in use = 1038915 APPENDIX P storage needed = 12913838 factor speedup = 1.9197E+00 solve speedup = 1.9378E+00 est. factor nonzeroes = 5.1432E+07 est. factor operations = 1.2099E+11 est. total factor nz. = 9.9666E+07 est. max. factor op. = 1.2099E+11 est. total factor op. = 2.3293E+11 est. max. factor nz. = 5.1432E+07 The first two rows reports the CPU and wall clock time for doing the symbolic factorization in terms of seconds. The next two are storage requirements for the symbolic factorization, of which the latter is the memory reserved for this. After this we have estimations of the speedup in the factorization and subsequent solve of the linear system of equations, this is a report from an MPP run on 2 processors. The last lines refer to the estimated requirement for storing and factorizing the system matrix, and distinguish between the local, total and maximum number of each of these two entries. This allows for determining the memory scaling in the case of an MPP run. Now LS-DYNA is in the position of reserving space for the factorization of the system matrix, and a report on the storage needed for this is given. symbolic storage 1 = 1038915 in-core numeric storg 1 = 62762269 out-of-core num. storg 1 = 13168676 symbolic storg 1 = 1.04 Mw in-core numericl storg 1 = 69.06 Mw out-of-core num. storg 1 = 14.51 Mw Here basically the same information is repeated, except for a slight increment in order to account for potential penalty when doing the actual factorization. The first is again the memory reserved for the symbolic factorization and the other two are the memory required to perform an in-core and out-of-core factorization, respectively. If the memory available is not sufficient for doing an in-core factorization, LS-DYNA warns about this and attempts to do an out-of-core factorization, which means that the hard disk is used to store information during factorization. If this warning appears it is recommended to restart the simulation and using more memory since out-of-core significantly (writing to disk is more expensive than accessing memory) adds to the wall clock time for solving the problem. If the memory for doing an out-of-core factorization is insufficient, LS-DYNA will terminate with an error message. Otherwise, memory is reserved and reported expanding memory to 77737167 linear eqn. solver numerical phase 1 meaning that the total amount of memory reserved at this point is roughly 78 Mwords. At this point a redistribution of the system matrix is performed and a short report is given on this APPENDIX P symbolic storage 2 = 1038915 in-core numeric storg 2 = 68238926 out-of-core num. storg 2 = 11553502 Now the actual factorization takes place and a report from this is given where the information of interest is CPU: factorization = 59.025 WCT: factorization = 50.151 act. factor nonzeroes = 5.1236E+07 act. factor operations = 1.2092E+11 act. max. factor nz. = 5.1236E+07 act. max. factor op. = 1.2092E+11 act. total factor nz. = 9.9666E+07 act. total factor op. = 2.3293E+11 which basically is the same information as from the symbolic factorization except that now it is the actual instead of the estimated values that is reported. Finally, the forward and backward substitutions are allocated for and performed. The information given is symbolic storage 3 = 1038915 in-core numeric storg 3 = 68299122 out-of-core num. storg 3 = 16476693 CPU: numeric solve = 0.191 WCT: numeric solve = 0.194 Concluding, the wall clock time for solving the system of linear equations is reported WCT: total imfslv_mf2 = 75.079 ELEMENTS AND MATERIALS Implicit Accuracy Implicit and explicit analysis differ in many respects, an important one is that the deformation during a single step is much larger in implicit than a typical one in explicit. In the context of elements and materials, the demand for stronger objectivity and higher accuracy in implicit is obvious. The notion of implicit executing the same algorithms as a corresponding explicit analysis is whence not adopted in general. This can optionally be further extended, using IACC = 1 to increase implicit accuracy on *CONTROL_ACCURACY will make selected elements strongly objective and enhance the accuracy for selected materials. For instance will finite rotations be represented exactly and fully iterative plasticity adopted. In addition, the flag applies to tied contacts as will be elaborated on below. Currently the following elements are supported for this option APPENDIX P Solid elements -2,-1,1,2 Shell elements 4,-16,16,23,24 Beam elements 1,2,9 and materials 24 and 123 use fully iterative plasticity. CONTACTS Contacts are probably among the hardest features to treat in a nonlinear implicit simulation. They are divided into the categories tied (bilateral) and sliding (unilateral) contact, and the characteristics of the two are quite different. Tied contacts are most often applied as constraints, only sometimes using a penalty formulation, and are fairly easy to deal with as they are only moderately nonlinear. In contrast, sliding contacts are exclusively implemented as penalty contacts and hard to deal with because of the unilateral condition. While the number of contacts, see *CONTACT, in LS-DYNA is abundant, we will here only present the few contacts that make most sense to use in implicit. Tied Contacts Tied contacts in implicit analysis should be accompanied with the Implicit Accuracy option, as this essentially reduces the number of relevant contacts to use to only six. These six contacts are *CONTACT_TIED_NODES_TO_SURFACE *CONTACT_TIED_NODES_TO_SURFACE_CONSTRAINED_OFFSET *CONTACT_TIED_NODES_TO_SURFACE_OFFSET *CONTACT_TIED_SHELL_EDGE_TO_SURFACE *CONTACT_TIED_SHELL_EDGE_TO_SURFACE_CONSTRAINED_OFFSET *CONTACT_TIED_SHELL_EDGE_TO_SURFACE_BEAM_OFFSET The first and fourth of these project the nodes on the slave side to the master surface, while the rest are offset contacts for which nodes will remain in place. The fourth, fifth and sixth constrain rotations while the others do not. The third and sixth are penalty based, while the others are constraint based. In sum, these six contacts cover most reasonable scenarios. The implicit accuracy option will in this context make these six tied contact strongly objective, and built-in intelligence will detect whether nodes contain rotations to constrain or not. A nice feature with the latter is that torsion is automatically applied with physical consistency, so it is for instance no problem to use single beams to model spotwelds between solid elements, and when using the same connection technique between shells the beam axial rotational degrees of freedom will be constrained to the APPENDIX P translational degrees of the shells and thus avoiding the relatively weak (and non- physical) drilling degree of freedom. This situation is depicted below. be The choice of contact depends on the situation, but from a conceptual point of view it should use for *CONSTRAINED_TIED_SHELL_EDGE_TO_SURFACE_CONSTRAINED_OFFSET most cases. The only problem then would be if complicated geometry results in termination due to overconstraining, for which a switch to the corresponding penalty is version motivated. See remarks in the LS-DYNA keyword manual for more information. *CONSTRAINED_TIED_SHELL_EDGE_TO_SURFACE_BEAM_OFFSET ok to Sliding Contact The choice of contact in this section is the Mortar contact as this seems to be best implicit contact algorithm when considering a combination of speed, accuracy and robustness. The Mortar contact features smoothness and continuity that is highly appreciated in implicit analysis, but is on the other hand expensive enough to not be recommended for explicit analysis. Many other contact algorithms are supported for implicit analysis and execute faster than the Mortar contact, but this is often seen when the infamous IGAP flag is set to default. This flag manipulates the stiffness matrix to the extent that accuracy may be deteriorated, and if used the results should be thoroughly checked. For Mortar contact IGAP has a different meaning as will be described IGAP. See remarks in the LS-DYNA keyword manual for more information. Basics The Mortar contact is activated by typically appending the suffix MORTAR to the automatic single surface, automatic surface to surface or forming surface to surface keywords. It can also be run as tied and tiebreak contacts. All Mortar contacts are segment to segment and penalty based and the tied and tiebreak contacts are always offset, i.e., the tie occurs on the outer surfaces of shells and not on the mid surfaces. For automatic contacts, edge contact with flat edges is always active. At this point, it possesses features that are of particular interest to implicit and that are not available for other contacts. It is supported in both SMP and MPP but the option MPP does not apply, and the SMP ignore flag applies. The SOFT flag does not apply, to summarize it is a contact algorithm especially intended for implicit analysis. Recommendations APPENDIX P For the forming contact the rigid tools must be meshed so that the normals are directed towards the blank, and contacts from above and below must be separated into two or more interfaces because contact can only occur from one side of the blank for a given contact interface. For the forming contact, rigid shells on the master side have no contact thickness. This is not the case for automatic contacts, here there are no restrictions on the mesh and even rigid shells have contact thickness. For all Mortar contacts, part or part set based slave and master sides are recommended although not mandatory. If the two sides in the contact interface have different stiffness, use the weak part as slave in order to get the best possible implicit convergence behavior. This is automatically taken care of in a single surface contact. Characteristics The contact pressure in the Mortar contact is a parabolic function of the penetration in combination with a cubic stiffening phase. In short, the contact stiffness depends on the slave side material and a characteristic length of the slave side segment. The characteristic length is for shells the shell thickness and for solids it is a median of the edges in the slave side of the contact interface, and the maximum penetration allowed is given as 95% of the average characteristic lengths on master and slave sides. For solids the definition of the characteristic length may have the consequence that the stiffness becomes unnecessarily high if some elements are much smaller than most, and stiffness adjustments may be necessary. Furthermore, the characteristic length also determines the maximum penetration as well as the search radius for finding contact pairs, for this reason the characteristic length can optionally be increased by assigning it on PENMAX on optional card B. In most cases it is expected that default value (=0.0) for this parameter will suffice. IGAP The contact stiffness is parabolic with respect to penetration up to a penetration depth corresponding to half of the maximum penetration. For IGAP = 1 it will remain parabolic for even larger penetrations but the user may increase IGAP which means APPENDIX P that the contact will stiffen for larger penetrations, in fact it will become cubic according to the picture above. The purpose of increasing IGAP could be to prevent the penetration from becoming larger than the maximum allowed penetration, because if convergence is attained with penetrations larger than this value this contact will be released in subsequent steps and the simulation is likely destroyed. Penetrations of this depth are likely to cause discontinuities along line searches and other discouraging phenomena. The user may of course scale the stiffness by increasing SFS but this also scales the stiffness for small penetrations and probably has a negative effect on convergence. Output for debugging Just as for implicit in general, Output is always a good thing to have when convergence starts deteriorating and considering the release of contact in the previous section, it would be interesting to know if penetrations are large enough for this to be a potential danger. First, initial penetrations are always reported in the message file(s), including the maximum penetration and how initial penetrations are to be handled. The latter depends on the value of the IGNORE flag and this is dealt with Initial Penetrations. In addition, by putting MINFO = 1 on *CONTROL_OUTPUT, LS-DYNA will report the absolute maximum penetration as well as the maximum penetration in percentage after each equilibrium. If the relative maximum penetration reaches above 99% a warning message is printed as this particular contact is close to being released. The output is exemplified in the following. Contact sliding interface 1 Number of contact pairs 527 Maximum penetration is 0.2447797E+00 between elements 306774 and 306672 Maximum relative penetration is 0.2266694E+02 % between elements 306742 and 306733 Contact sliding interface 2 Number of contact pairs 16209 Maximum penetration is 0.5027643E+00 between elements 219492 and 94935 Maximum relative penetration is 1.0366694E+02 % between elements 219492 and 94935 *** Warning Penetration is close to maximum before release This percentage value should ideally be kept below some 90 % to have some sort of comfort margin. There are three ways to reduce maximum relative penetrations, and these are (i) to increase IGAP, (ii) to increase SST for solids or (iii) to increase SFS. Note that by increasing SST for solids the contact stiffness will automatically be decreased, APPENDIX P and this should be accompanied by increasing SFS by the square of the fraction increase of SST. That is, if SST is doubled then SFS should be increased four times, and if SST is tripled then SFS should be increased nine times, and so on. In this case even IGAP may have to be increased by some amount if being larger than unity in the first place. Initial Penetrations As mentioned above, initial penetrations are always reported in the message file(s), including the maximum penetration and how initial penetrations are to be handled. The IGNORE flag governs the latter and the options are IGNORE < 0 IGNORE = 0 IGNORE = 1 IGNORE = 2 IGNORE = 3 IGNORE = 4 Same functionality as the corresponding absolute value, but contact between segments belonging to the same part is ignored completely Initial penetrations will give rise to initial contact stresses, i.e., the slave contact surface is not modified Initial penetrations will be tracked, i.e., the slave contact surface is translated to the level of the initial penetrations and subsequently follow the master contact surface on separation until the unmodified level is reached Initial penetrations will be ignored, i.e., the slave contact surface is translated to the level of the initial penetrations, optionally with an initial contact stress governed by MPAR1 Initial penetrations will be removed over time, i.e., the slave contact surface is translated to the level of the initial penetrations and pushed back to its unmodified level over a time determined by MPAR1 Same as IGNORE = 3 but it allows for large penetrations by also setting MPAR2 to at least the maximum initial penetration The use of IGNORE depends on the problem, if no initial penetrations are present there is no need to use this parameter at all. If penetrations are relatively small in relation to the maximum allowed penetration, then IGNORE = 1 or IGNORE = 2 seems to be the appropriate choice. For IGNORE = 2 the user may specify an initial contact stress small enough to not significantly affect the physics but large enough to eliminate rigid body modes and thus singularities in the stiffness matrix. The intention with this is to constrain loose parts that are initially close but not in contact by pushing out the contact surface using SFST and applying the IGNORE = 2 option. It is at least good for debugging problems with many singular rigid body modes. IGNORE = 3 is the Mortar interference counterpart, used for instance if there is a desire to fit a rubber component in a structure. With this option the contact surfaces are restored linearly in time from the beginning of the simulation to the time specified by MPAR1. A drawback with IGNORE = 3 is that initial penetration must be smaller than half the characteristic length of the contact or otherwise they will not be detected in the first place. For this reason IGNORE = 4 was introduced where initial penetrations may be of arbitrary size, but it requires that the user provides crude information on the level of penetration of the contact interface. This is done in MPAR2 which must be larger than the maximum APPENDIX P penetration or otherwise and error termination will occur. IGNORE = 4 only applies to solid elements at the moment. When eliminating penetrations by simulation for models with many parts, some parts may contain thin members that cause spurious self-contacts. These may be difficult to work around by only adjusting contact parameters, but fortunately there is rarely any loss of generality in ignoring contact within parts completely since those are usually not of interest in such a context. The option IGNORE < 0 was implemented for this purpose and is a way to approach this problem. Damping Damping can be activated in dynamic implicit analysis using VDC. A problem with contact damping in implicit is that the time step is usually large enough to not resolve the time in contact to get the desired damping effect. Often the situation becomes even worse, it is therefore not recommended to use damping. TROUBLESHOOTING CONVERGENCE PROBLEMS Convergence of the nonlinear equilibrium iteration process presents one of the greatest challenges to using the implicit mode of LS-DYNA. At risk of repeating what has already been mentioned, below are some useful troubleshooting approaches. Eigenvalue Analysis Many convergence problems in static implicit analysis are caused by unconstrained rigid body modes. These are created when an insufficient number of constraints are applied to the model, or when individual model parts are left disconnected. Eigenvalue analysis is an excellent diagnostic tool to check for these problems, both initially and at critical points in the simulation. The procedure for performing an eigenvalue analysis was discussed Singularities and Eigenvalue Analysis. D3Iter Plot Database To diagnose convergence trouble which develops in the middle of a simulation, get a picture of the deformed mesh. Adjust the d3plot output interval to produce an output state after every step leading up to the problematic time. An additional binary plot database named “d3iter” is available which shows the deformed mesh during each equilibrium iteration. This output is activated by D3ITCTL = 1 to activate d3iter plot database on *CONTROL_IMPLICIT_SOLUTION. View this database using LS-PrePost to detect abnormal displacements. The problem may become obvious, especially as deformation is magnified. If not, there is yet another flag to activate to get the residual forces into both this database as well as d3plot for fringing. Setting APPENDIX P RESPLT = 1 to get residual data to binary databases on *DATABASE_EXTENT_BINARY will do just that. With this option the residual forces are output to the d3plot and d3iter databases for fringing under the “NdV” menu. This is a great tool for locating areas in the model where the residual forces are not being reduced to a satisfactory level and take appropriate actions. Taking Advantage of ASCII Information If requested through Output on *CONTROL_IMPLICIT_SOLUTION and Output for debugging on *CONTROL_OUTPUT, a lot can be drawn from the information in the message file(s). This may be considered as a piece of advanced topic but may become useful in due time. Residual Norm Starting with the nonlinear output diagnostics, the following basic principle should be held in mind; if the residual norm is zero, the problem is solved. So it all comes down to make this number (11) small enough to trust the results. Therefore we suggest to monitor the residual norm and interpret it as an indicator of whether the convergence characteristics is good. Hopefully you would see this number decrease with implicit iterations and finally reach a relatively small number at convergence. Although it may (and will) increase on occasion, the trend should be a decreasing one. If this is a problem from the get-go, and you checked the model integrity through Singularities and Eigenvalue Analysis and common practice, it may be that a feature is not properly supported in implicit. 𝑒 Line search not solvable Acceptable interval 𝑠 𝑠 = 1 Smooth force, well behaved line search Discontinuous force, zero acceptable interval, indicates Line Search APPENDIX P Another thing to look at is the line search convergence (9), as the relatively loose line search convergence tolerance should render a reasonably small number of line search iterations. A rule of thumb would be less than 10, at most 20. If more is used, or if the line search does not converge, there may be something in the model causing a jump in the residual forces. This is not supposed to happen in implicit, and may suggest a bug. Either of the two following scenarios for a feature discontinuity (and many line search iterations) is possible •The line search step size becomes ridiculously small, and the current residual norm (7) is not approaching the initial one (3). •The interval in which the optimal step is to be found (8) becomes ridiculously small, and the residual norm on the left and right interval points are not ap- proaching eachother. This situation is depicted in the figure above (dashed line). Many line search iterations can of course be due to high nonlinearities but if the above is observed it should probably be investigated, for instance by trying to identify model features that may be causing the bad behavior. If it is obvious that a discontinuity exist, like if the step size goes down to ~1−100 or the interval size becomes zero, and it is not due to a model error, please send a bug report. Stretching for Convergence If the problem runs fine for a significant number of load/time steps with subsequent convergence issues, then the information received up to this point may be used intelligently and suggest a different (unorthodox) implicit strategy. To justify the approach, we begin by recalling that the convergence is detected by the following numbers becoming small; 𝑑 = ‖∆𝒖‖ (displacement norm), 𝑟 = ‖𝑹‖ (residual norm) and 𝑒 = ∣𝑹𝑇∆𝒖∣ (energy norm). But all these numbers are linked through the General, 𝑲∆𝒖 = 𝑹, so if 𝑲 reasonably “nice” at all times it doesn’t matter which numbers we use for detecting convergence. A mathematical way to state this is; if the condition number of 𝑲 is “good”, then all the norms are equivalent throughout the solution process. An intuitive statement would be to say that the problem is only moderately nonlinear, and convergence is usually never a problem. But, what happens if the properties of 𝑲 are not that nice, or if 𝑲 shifts character every time it is reformed? This is sort of saying that the problem is highly nonlinear, for instance due to frequent change of contact state or onsets/offsets of plasticity. In those cases the equivalence between 𝑑 and 𝑟 is lost, and typically an oscillatory behavior of the displacement norm is observed even though the residual norm is reducing, which in turn may lead to potential convergence problems just because the displacement criterion cannot be satisfied. Or equally bad, it could lead to Premature Convergence just by the coincidence that the displacement norm happens to become small. In those cases we essentially want to come up with a strategy where the displacement criterion is taken out of the convergence check and instead detect convergence based on residual only. So assume we have say 10 converged states, after which the convergence problems begin. Then we can look at what the residual norm is for each of these converged states (11), for instance we may see the sequence APPENDIX P Step 1, residual norm 2859 Step 2, residual norm 1581 Step 3, residual norm 2119 Step 4, residual norm 2511 Step 5, residual norm 11570 Step 6, residual norm 4904 Step 7, residual norm 3586 Step 8, residual norm 3157 Step 9, residual norm 3315 Step 10, residual norm 2825. For each of these steps we may validate the results, by post-processing contact force curves, checking force/moment balance etc., in LS-PrePost, and usually there is a correlation between “good results” and small residual norms. Step 5 above is for instance an outlier and may be associated with a prematurely converged step, something that can be confirmed or rejected from looking at the result. The goal with these observations is to establish a reasonable residual norm for which we can safely say that the results are good, and the numbers above indicates that 3000 may be a good candidate. The strategy is then to simply put DCTOL = 1.e-16 to ignore the displacement and set ABSTOL = -3000, which means we can be assured that convergence will not be detected until the residual norm is below 3000, and we “know” from having learned about the problem that this will yield good results. It should be mentioned that this may not work if the character (force level) changes significantly later on in the simulation, as 3000 then may not be the number we would trust. Contacts Continuing with the Output for debugging, a general rule is that there should be no warnings of large penetrations and preferably the maximum relative penetration should be below 90%. These numbers can be monitored after each load/time step. If large penetrations occur, either increase IGAP or contact stiffness, whatever makes most sense, but first make sure that the converged step is really converged (no Premature Convergence) by monitoring the residual forces and checking results as indicated above. CHECKLIST So, to summarize Activate implicit by setting IMFLAG = 1 on *CONTROL_IMPLICIT_GENERAL •Set DT0 to a reasonable initial time step APPENDIX P Check possible singularities in an eigenvalue analysis by requesting NEIG eigenvalues on *CONTROL_IMPLICIT_EIGENVALUE •Find a way to constrain spurious modes Initially use dynamic analysis if rigid body modes are present in a static problem by setting IMASS = 1 on *CONTROL_IMPLICIT_DYNAMICS •Use TDYBIR, TDYDTH and TDYBUR •Use numerical damping by putting GAMMA = 0.6 and BETA = 0.38 Only activate geometric stiffness contribution as a last resort, except for arc length methods Use default BFGS parameters ILIMIT and MAXREF on *CONTROL_IMPLICIT_SOLUTION •Increase or decrease ILIMIT based on convergence characteristics •Use full Newton (ILIMIT = 1) for hard problems •Keep MAXREF to a reasonably low number Use default convergence tolerances DCTOL, ECTOL and RCTOL on *CONTROL_IMPLICIT_SOLUTION •ABSTOL may be set to 1.e-20 to prevent premature convergence •Relaxing DCTOL may not necessarily result in better convergence •Future strategy may be to focus on residual Activate automatic time stepping on *CONTROL_IMPLICIT_AUTO •Set DTMAX to a number that resolves features of interest Contacts Material nonlinearities Frequencies Use default line search method on *CONTROL_IMPLICIT_SOLUTION •Switch to LSMTD = 5 if hard problem (typically rubbers) •Don’t change LSTOL Use at least NLPRINT = 2 on *CONTROL_IMPLICIT_SOLUTION to get conver- gence diagnostics into log files •Use NLPRINT = 3 to thoroughly track the residual norm and monitor line search behavior if debugging model is necessary Use *CONTROL_IMPLICIT_SOLVER only in special occasions Set D3ITCTL = 1 on *CONTROL_IMPLICIT_SOLUTION to get a database with Newton iterates when debugging a model •Complement this with RESPLOT = 1 on *DATABASE_EXTENT_BINARY to get the possibility to fringe the residual force vector For forming Mortar contact, make sure •Tools are oriented towards the blank APPENDIX P •Contact on top and bottom of blank are separated among contact interfaces Use part (set) definitions of slave and master in Mortar contact Always use weak part as slave in a Mortar contact definition to get best possible convergence Set SST to a reasonable characteristic length for slave side consisting of solid elements •With this option, separate solids and shells into different contact interfaces in order to not manipulate the contact thickness for shells If penetrations are large, activate penetration diagnostics on *CONTROL_CONTACT To avoid release of contact pairs, either •Increase stiffness scaling factor SFS •Increase IGAP for progressive stiffness increase •Increase SST for solids while at the same time increasing SFS Use IGNORE appropriately to deal with initial penetrations •Check initial penetrations in message file Don’t use contact damping APPENDIX Q APPENDIX Q: User Defined Weld Failure The addition of a user weld failure subroutine into LS-DYNA is relatively simple. The UWELDFAIL subroutine is called every time step when OPT = 2 is specified in MAT_- SPOTWELD. As data, the identification number for the spotweld material, six constants specified in the input by thfe locations NRR through MTT, the radius of the cross section of the spotwelds, the current time, and the current values of the resultants for the spotwelds, which are stored in array STRR, are passed to the subroutine. The subroutine loops over the welds from LFT through LLT, and sets the values of the failure flag array FLAG. SUBROUTINE UWELDFAIL(IDWELD,STRR,FAIL,FIBL,CM,TT,LFT,LLT) C****************************************************************** C| LIVERMORE SOFTWARE TECHNOLOGY CORPORATION (LSTC) | C| ------------------------------------------------------------ | C| COPYRIGHT 2002 JOHN O. HALLQUIST, LSTC | C| ALL RIGHTS RESERVED | C****************************************************************** C C*** SPOTWELD FAILURE ROUTINE C C*** LOCAL COORDINATES: X IS TANGENT TO BEAM, Y & Z ARE NORMAL C C*** VARIABLES C IDWELD ---- WELD ID NUMBER C STRR ------ STRESS RESULTANTS C (1) AXIAL (X DIRECTION) FORCE C (2) Y SHEAR FORCE C (3) Z SHEAR FORCE C (4) MOMENT ABOUT Z C (5) MOMENT ABOUT Y C (6) TORSIONAL RESULTANT C FAIL ------ FAILURE FLAG C = 0 NOT FAILED C = 1 FAIL ELEMENT C FIBL ------ LOCATION (1,*) GIVES THE SPOTWELD DIAMETER C CM -------- 6 CONSTANTS SUPPLIED BY USER C TT -------- CURRENT SIMULATION TIME C LFT,LLT --- DO-LOOP RANGE FOR STRR C DIMENSION IDWELD(*),STRR(6,*),FAIL(*),CM(*),FIBL(5,*) C C RETURN END APPENDIX R APPENDIX R: User Defined Cohesive Model The addition of a user cohesive material subroutine into LS-DYNA is relatively simple. The UMATiC subroutine is called every time step where i ranges from 41 to 50. Input for the material model follows the *MAT_USER_DEFINED_MATERIAL definition. The user has the option of providing either a scalar or vectorized subroutine. As discussed in the Remarks for the user-defined material, the first two material parameters are reserved to specify how the density is treated and the number of integration points required for the failure of the element. The cohesive model calculates the tractions on the mid-surface of the element as a function of the differences of the displacements and velocities of the upper (defined by nodes 5-6-7-8) and lower surfaces (defined by nodes 1-2-3-4). The displacements, velocities, and the calculated tractions are in the local coordinate system of the element, where the first two components of the vectors are in the plane of the mid-surface and the third component is normal to the mid-surface. A stiffness must also be calculated by the user for the explicit time step calculation in LS-DYNA. This stiffness must provide an upper bound on the stiffness in all three directions. The material fails at an integration point when ifail=.true. For an element to be deleted from the calculation, the number of integration points specified by the second material parameter must fail. If the second parameter is zero, elements cannot fail regardless of the specification of IFAIL in the user-defined material input. For example, the user may choose to reject an implicit step is the displacement increment is too For implicit analysis, the subroutine is called with maketan=.true. and the user must provide the elastic moduli in the three local directions in the respective diagonal terms of the dsave array. The parameter reject, if set to .true. by the user, will signal to LS- DYNA that the current implicit iteration is unacceptable. For example, the user may choose to reject an implicit step if the traction changes too much from the last time step. In this situation, LS-DYNA will print a warning message `Material model rejected current iterate’ and retry the step with a smaller time step. If chosen carefully (by way of experimenting), this may result in a good trade-off between the number of implicit iterations per step and the step size for overall speed. The following example is a vectorized model with two elastic constants and failure: subroutine umat41c(idpart,cm,lft,llt,fc,dx,dxdt,aux,ek, & ifail,dt1siz,crv,nnpcrv,nhxbwp,cma,maketan,dsave,ctmp,elsiz, & reject,ip,nip) include 'nlqparm' APPENDIX R c*** vector cohesive material user model example c c*** variables c idpart ---- Part ID c cm -------- material constants c lft,llt --- start and end of block c fc -------- components of the cohesive force c dx -------- components of the displacement c dxdt ------ components of the velocity c aux ------- history storage c ek -------- max. stiffness/area for time step calculation c ifail ----- =.false. not failed c =.true. failed c dt1siz ---- time step size c crv ------- curve array c nnpcrv ---- # points per curve for crv array c nhxbwp ---- internal element id array, lqfinv(nhxbwp(i),2) c gives external element id c cma ------- additional memory for material data defined by c LMCA in 2nd card, 6th field of *MAT_USER_DEFINED c maketan --- true for implicit c dsave ----- material stiffness array, define for implicit c ctmp ------ current temperature c elsiz ----- characteristic element size (=sqrt(area)) c reject ---- set to .true. if this implicit iterate is c to be rejected for some reason (implicit only) c ip -------- integration point number c nip ------- total number of integration points c c*** dx, dxdt, and fc are in the local coordinate system: c components 1 and 2 are in the plane of the cohesive surface c component 3 is normal to the plane c c*** cm storage convention c (1) =0 density is per area c =1 density is per volume c (2) number of integration points for element deletion c =0 no deletion c (3:48) material model constants c logical ifail,maketan,reject dimension cm(*),fc(nlq,*),dx(nlq,*),dxdt(nlq,*), & aux(nlq,*),ek(*),ifail(*),dt1siz(*),crv(101,2,*), & nhxbwp(*),cma(*),dsave(nlq,6,*),ctmp(*),elsiz(*) integer nnpcrv(*) c c et=cm(3) en=cm(4) eki=max(et,en) fcfail=cm(5) c do i=lft,llt fc(i,1)=et*dx(i,1) fc(i,2)=et*dx(i,2) fc(i,3)=en*dx(i,3) ek(i)=eki ifail(i)=fc(i,3).gt.fcfail enddo c if(maketan) then do i=lft,llt dsave(i,1,1)=et dsave(i,2,1)=0. dsave(i,3,1)=0. dsave(i,1,2)=0. APPENDIX R dsave(i,2,2)=et dsave(i,3,2)=0. dsave(i,1,3)=0. dsave(i,2,3)=0. dsave(i,3,3)=en enddo endif return end The second example implements the Tveergard-Hutchinson cohesive model with failure in both the vectorized (UMAT42C) and scalar (UMAT43C) forms. Note the LFT and LLT are passed to the scalar version, however their value is zero. subroutine umat42c(idpart,params,lft,llt,fTraction,jump_u,dxdt, & aux,ek,ifail,dt1siz,crv,nnpcrv,nhxbwp,cma,maketan,dsave,ctmp,elsiz, & reject,ip,nip) include 'nlqparm' c c*** vector cohesive material user model example c c Tveergard-Hutchinson model based on: c tahoe/src/elements/cohesive_surface/cohesive_models/TvergHutch3DT.cpp c c the declaration below is processed by the C preprocessor and c is real*4 or real*8 depending on whether LS-DYNA is single or double c precision c REAL L,jump_u logical ifail,maketan,reject dimension params(*),fTraction(nlq,*),jump_u(nlq,*),dxdt(nlq,*), & aux(nlq,*),ek(*),ifail(*),dt1siz(*),crv(101,2,*), & nhxbwp(*),cma(*),dsave(nlq,6,*),ctmp(*),elsiz(*) integer nnpcrv(*) c fsigma_max=params(3) fd_c_n=params(4) fd_c_t=params(5) fL_1=params(6) fL_2=params(7) fpenalty=params(8) c fK=fpenalty*fsigma_max/(fL_1*fd_c_n) c fac=min(fd_c_n/fd_c_t**2,1./fd_c_n) c do i=lft,llt u_t1 = jump_u(i,1) u_t2 = jump_u(i,2) u_n = jump_u(i,3) c r_t1 = u_t1/fd_c_t r_t2 = u_t2/fd_c_t r_n = u_n/fd_c_n L = sqrt(r_t1*r_t1 + r_t2*r_t2 + r_n*r_n) c if (L .lt. fL_1) then sigbyL=fsigma_max/fL_1 APPENDIX R else if (L .lt. fL_2) then sigbyL = fsigma_max/L else if (L .lt. 1.) then sigbyL = fsigma_max*(1. - L)/(1. - fL_2)/L else sigbyL = 0.0 ifail(i)=.true. endif c fTraction(i,1) = sigbyL*r_t1*(fd_c_n/fd_c_t) fTraction(i,2) = sigbyL*r_t2*(fd_c_n/fd_c_t) fTraction(i,3) = sigbyL*r_n c c penetration if (u_n .lt. 0) fTraction(i,3)=fTraction(i,3)+fK*u_n c c approximate stiffness for time step if (u_n .lt. 0) then ek(i)=fac*sigbyL+fK else ek(i)=fac*sigbyL endif c if (maketan) then dsave(i,1,1)=sigbyL/fd_c_t*(fd_c_n/fd_c_t) dsave(i,2,1)=0. dsave(i,3,1)=0. dsave(i,1,2)=0. dsave(i,2,2)=sigbyL/fd_c_t*(fd_c_n/fd_c_t) dsave(i,3,2)=0. dsave(i,1,3)=0. dsave(i,2,3)=0. dsave(i,3,3)=sigbyL/fd_c_n if (u_n.lt.0) dsave(i,3,3)=dsave(i,3,3)+fk endif enddo c return end c c c subroutine umat43c(idpart,params,lft,llt,fTraction,jump_u,dxdt, & aux,ek,ifail,dt1siz,crv,nnpcrv,nhxbwp,cma,maketan,dsave,ctmp,elsiz, & reject,ip,nip) c c*** scalar cohesive material user model example c c Tveergard-Hutchinson model based on: c tahoe/src/elements/cohesive_surface/cohesive_models/TvergHutch3DT.cpp c c the declaration below is processed by the C preprocessor and c is real*4 or real*8 depending on whether LS-DYNA is single or double c precision c REAL L,jump_u logical ifail,maketan,reject dimension params(*),fTraction(nlq,*),jump_u(nlq,*),dxdt(nlq,*), & aux(nlq,*),ek(*),ifail(*),dt1siz(*),crv(101,2,*), & nhxbwp(*),cma(*),dsave(nlq,6,*),ctmp(*),elsiz(*) integer nnpcrv(*) c fsigma_max=params(3) fd_c_n=params(4) fd_c_t=params(5) fL_1=params(6) APPENDIX R fL_2=params(7) fpenalty=params(8) c fK=fpenalty*fsigma_max/(fL_1*fd_c_n) c fac=min(fd_c_n/fd_c_t**2,1./fd_c_n) c u_t1 = jump_u(1) u_t2 = jump_u(2) u_n = jump_u(3) c r_t1 = u_t1/fd_c_t r_t2 = u_t2/fd_c_t r_n = u_n/fd_c_n L = sqrt(r_t1*r_t1 + r_t2*r_t2 + r_n*r_n) c if (L .lt. fL_1) then sigbyL=fsigma_max/fL_1 else if (L .lt. fL_2) then sigbyL = fsigma_max/L else if (L .lt. 1.) then sigbyL = fsigma_max*(1. - L)/(1. - fL_2)/L else sigbyL = 0.0 ifail=.true. endif c fTraction(1) = sigbyL*r_t1*(fd_c_n/fd_c_t) fTraction(2) = sigbyL*r_t2*(fd_c_n/fd_c_t) fTraction(3) = sigbyL*r_n c c penetration if (u_n .lt. 0) fTraction(3)=fTraction(3)+fK*u_n c c approximate stiffness for time step if (u_n .lt. 0) then ek=fac*sigbyL+fK else ek=fac*sigbyL endif c if (maketan) then dsave(1,1)=sigbyL/fd_c_t*(fd_c_n/fd_c_t) dsave(2,1)=0. dsave(3,1)=0. dsave(1,2)=0. dsave(2,2)=sigbyL/fd_c_t*(fd_c_n/fd_c_t) dsave(3,2)=0. dsave(1,3)=0. dsave(2,3)=0. dsave(3,3)=sigbyL/fd_c_n if (u_n.lt.0) dsave(3,3)=dsave(3,3)+fk endif return end APPENDIX S APPENDIX S: User Defined Boundary Flux A user defined boundary flux interface is provided in LS-DYNA where it is possible to define the thermal heat flux (power per surface area) in or out of a surface segment as an arbitrary function of temperature and history. The user may associate history variables with each individual flux interface and also use load curves. The user flux interface is invoked using the keyword *BOUNDARY_FLUX_OPTION. This is accomplished with the parameter NHISV. When it is defined with a value greater than 0, the user subroutine subroutine usrflux(fl,flp,…) is called to compute the flux (fl) defined as heat (energy) per time and per surface area. Other parameters that are passed to the user flux subroutine include the segment nodal temperatures at the previous (T0) and current time (T1), the segment nodal coordinates and the time integration parameter α. Also, the current thermal simulation time t, the time step Δt and average segment temperature (Tα) at time t+αΔt is provided together with the curve array for accessing defined load curves in the keyword input file. For computing load curve values, note that load curve IDs need to be transformed to internal numbers or the subroutine crvval should be used, see the appendix on user defined materials for details. The segment coordinates available in the subroutine are such that the outward normal vector follows the well-known right-hand rule, thus segments corresponding to the lower surface of thick thermal shells are reversed before passed to the subroutine. For shells in general, the segment connectivity should follow the connectivity of the actual shell element to avoid problems. Optionally, the user may define the derivative of the flux fl with respect to the average segment temperature (Tα) at time t+αΔt, flp. This value is used in the nonlinear thermal solver for assembling the correct stiffness matrix and must be set by the user. If possible, it is recommended to use a value that reflects the nonlinearity of the flux model, otherwise the value 0 should be used. An array of history variables, identical with the input parameters defined in the keyword input file, are passed to the subroutine that can be updated with time or kept constant throughout the simulation. An example of usage would be to integrate the flux with time to keep track of the dissipated energy per surface area in order to simulate the effects of spray cooling in hot-stamping. APPENDIX S time) (input) subroutine usrflux(fl,flp,x,tnpl,tnl,nodes, . alpha,atime,atemp,dt,time,fhsv,nfhsv,crv) C****************************************************************** C| LIVERMORE SOFTWARE TECHNOLOGY CORPORATION (LSTC) | C| ------------------------------------------------------------ | C| COPYRIGHT © 2007 JOHN O. HALLQUIST, LSTC | C| ALL RIGHTS RESERVED | C****************************************************************** c c User subroutine for boundary thermal flux c c Purpose: To define thermal flux parameter (heat per surface area and c c c Variables: c c fl = flux intensity (output) c flp = flux intensity derivative wrt atemp (output) c x(3,nodes) = global segment coordinates (input) c tnpl(nodes) = temperatures at time time (input) c tnl(nodes) = temperatures at time time-dt (input) c nodes = number of nodes in segment (3,4 or 6) (input) c alpha = time integration parameter (input) c atime = time+(alpha-1)*dt c atemp = average segment temperature at time atime c dt = time step size (input) c time = time at which the new temperature is sought (input) c fhsv(nfhsv) = flux history variables (input/output) c nfhsv = number of flux history variables for this segment c c crv = curve array (input) c include 'nlqparm' dimension x(3,*),tnpl(*),tnl(*) dimension fhsv(*),crv(lq1,2,*) c c Define flux by linear convection c that optionally decays (in an ad-hoc way) as power c dissipates from surface c c fhsv(1) = convection coefficient c fhsv(2) = ambient temperature c fhsv(3) = total amount of energy per surface area available c fhsv(4) = dissipated energy per surface area at current c hcon=fhsv(1) tinf=fhsv(2) flin=hcon*(tinf-atemp) if (nfhsv.gt.2) then q=(1.-fhsv(4)/fhsv(3))/ . (1.+.5*dt*flin/fhsv(3)) flp=-q*hcon if (q.gt.1.) then q=1. flp=-hcon elseif (q.lt.0.) then q=0. flp=0. endif fl=q*flin fhsv(4)=fhsv(4)+dt*.5*fl fhsv(4)=min(fhsv(3),fhsv(4)) else fl=flin flp=-hcon endif APPENDIX S c return end APPENDIX T: Metal Forming Glossary A TYPICAL DRAW DIE ENGINEERING PROCESS Clay models of a new vehicle are scanned and the outer shell surfaces are created in a design studio. Body-in-white engineers and designers are responsible to create all the inner parts and various structure and underbody parts. Flanges are created on outer surface parts to be joined with the inner panels. These parts are typically created in the car axis; with global X-axis runs from the front to the back along the car’s center line, global Y-axis from the driver side to the passenger side and Z-axis going straight up. During the clay design and shaping, simultaneous and multidisciplinary engineering may be practiced involving divisions/departments from design, engineering and manufacturing. Material suppliers may also be involved in this stage for consultation if advanced materials are to be applied. Multidisciplinary involvement in this early stage of a vehicle development allows manufacturing engineers to capture any part designs with “no make” conditions that would be costly if they were allowed to proceed to a later stage; while design envelopes can be pushed to their maximum potential within the state-of-art manufacturing capabilities. During the advance feasibility phase, parts from the design studio are processed quickly to go through an engineering process involving mainly the process engineer and FEA simulation engineer. Addendum and binder are roughly built in order to conduct a reliable draw die simulation. The exact process eventually would be used to build the die may not yet be established, therefore similar processes from knowledge base are used as references. Rarely are secondary dies (all dies except draw die) simulated. The main task here is to provide some quick assessment of the part’s manufacturability through fast design/engineering iterations. During the hard die design and construction phase, stamping manufacturing processes (some in three dimensional) are established, by referring to existing knowledge base, with necessary modifications needed for the current part design, and with the limits of manufacturing equipment such as press type, shut height, maximum tonnage and automation, etc. The stamping process includes the number of dies (to make a complete part of the final shape), part tipping, draw height, trimming (direct or aerial), flanging, springback compensation requirements, etc. Not all areas of the part may be formed to its final shape in one draw die. Some involve redraw die if one area of the part is especially deep compared to the rest of the part, which may otherwise cause uncontrollable wrinkles, splits, or exceed the draw height limit without the redrawing. Some areas of the part (which may have “undercut” or “die locked” conditions) may be unfolded to the addendum, then trimmed and flanged in a flanging die later. A typical APPENDIX T example of such can be found along the hood line of a fender outer. There may be multiple trimming and flanging dies, since not all areas of the drawn panel may be feasible for trimming or flanging all in one trim or flanging die. Referring to Figure 63-1, a typical draw die development process flow for an outer part is illustrated. The part is tipped from the global car axis to a ‘draw die’ axis, which takes into account of balancing the internal draw angles over the entire part, and minimizing the overall draw height, etc. Hem flanges are unfolded off the part breakline (Figure 63-1) in one of the following ways: 1)Tangent extension of the part surface, 2)Horizontal surface, 3)Vertical down-standing surface, 4)Any angled surface between horizontal and vertical surface, 5)To the addendum surfaces to be designed; in this case, the unfolding will happen after the addendum design is complete. Flange unfold must take into account the trimming condition later in the trim dies. Direct trim represents the trim steel going down in a draw direction (vertical); while aerial (cam) trim steel covers all other directions, driven by a ‘cam driver’ driven further by the vertical downward motion of the trim die. There are specific trim angle requirements for direct and aerial trim operations. Next, the part boundary is smoothed, filling up any gaps, holes and sharp features. The boundary will likely be modified later during the addendum build. Binder is created, based on the unfolded part boundary and overall part curvature. A developable binder surface, which consists of planes, cylindrical surfaces or a combination of both, is preferred; however, in some cases a doubly curved binder surface (undevelopable surface) must be designed for the purpose of reducing the draw depth at critical locations for material utilization, alleviating thinning, or both. Theoretical punch opening line (P.O. line, Detail #2 in Figure 63-1) can be offset from the smoothed part boundary in the plane normal to the draw axis, projected to the binder surface in the draw direction; some smoothing of the P.O. lines may be required. Generally, the finished P.O. lines should be consisted of mostly straight lines and radii, with generous transition among corners. P.O. lines do not follow tight corners, avoiding formation of wrinkles during the draw. In addition, design of P.O. lines must take into consideration the material utilization issue, especially in the blank sizing critical locations. Once P.O. lines design is complete, binder surfaces inside of the P.O. are trimmed and the remaining binder surface design is sent for binder closing simulation. Given a blank initial shape, simulation of the binder closing action can determine the quality of the binder design. Typically, for exterior outer panels, no buckles or wrinkles are allowed during the closing; for inner panels, some wrinkles are acceptable, or even desirable, depending on the part shape. Lower punch/post support may be introduced to reduce the draw height, alleviate thinning, or remove the initial blank drape into the binder cavity. Based on the binder closing simulation results, unacceptable binder design is sent back for rework, and the satisfactory binder design proceeds into the next step of addendum APPENDIX T build, which is used to fill the space between the part boundary and binder surface. It is noted that the P.O. lines may need to be adjusted during the addendum design. The trimming condition may also be affected and modified during the addendum design. Next, draw simulation ensues, assessing the overall formablity of the draw design. If quality targets are not achieved in the simulation, the process may go all the way back to the tipping for redesign/reprocess; otherwise successful simulation will direct the draw surface design to the next stage of draw die structure design. TYPES OF DRAW DIES There are many different types of draw dies used to punch the part to their intended shape, as shown in Figure 63-2. They basically can be divided into either single action or double action dies. Specifically (names may vary among different companies), 1)Air draw ― Single action. It is a 3-piece die system with 1 piece upper (cavity) and 2-piece (binder and punch/post) lowers. The upper cavity (driven by press ram) moves down in one action to close with the lower binder, and then closes with the lower punch to draw the part to the home position. The lower binder is either sitting on an air cushion through pins that go through the press bed, or directly on nitrogen cylinders arranged uniformly between the bottom of the binder structure and the press bed; the punch is fixed onto the press bed. This is the most popular draw type, mainly because of its speed and efficiency. Its limitation includes a maximum draw height of 10”. 2)Toggle draw ― Double action. It is a 3-piece die system with 2-piece upper (binder and punch) and 1 piece (cavity) lower. Upper binder, driven by the outer ram of the press, moves down to clamp the blank with the lower cavity; then the upper punch, driven down by the inner ram, closes with the lower cavity to complete the draw. Since this adds another action, it is slower than the air draw; howev- er, this type of draw die is well suited to control the wrinkles created during the forming of difficult part, such as liftgate and door inner. Furthermore, this type of draw has a relatively large draw height, which is limited only by the press. 3)Air draw with pressure pad ― Single action. This is very similar to 1), except an additional pressure pad, driven by nitrogen cylinders mounted on the upper die structure, closes first with the lower punch, then the entire upper comes down to finish the draw. This is similar to 1) in efficiency. 4)Stretch Draw (four piece) ― Double action. It is a 4-piece die system with 2-piece uppers (upper binder and punch) and 2-piece lowers (lower binder and cavity). Upper binder moves down to close with lower binder, moving together for a certain distance (up to 2”), then upper punch comes down to completely close with lower cavity. Finally the binders move down together to their home posi- tion. This process is not used as often as 1), 2) and 3), however, it is very capable in forming difficult inner parts, especially those prone for wrinkles, such as liftgate inner, door inner and floor pan. Since there is a ‘pre-stretch’ action with APPENDIX T the binders clamping the blank and moving down together, strain path change in the part during the forming is expected. This is the slowest draw type. 5)Crash Form Die ― Single action. It is a 2-piece die system with no upper or binders. Upper and lower tool takes the same shape, with upper moving down to close with the lower tool. This is obviously a very simple die, which can handle simple parts, with not too much draw depth variation (near constant draw depth all around). TYPES OF FLANGING DIES There are three types of flanging dies, as shown in Figure 63-3. All three types have a fixed lower (trim) post upon which the drawn (or partially trimmed part) is sitting, and a pressure pad (or multiple pads) which holds the part (which is loaded onto the post in a vertical direction) in place against the post. In a direct flanging process, the flanging steel (Figure 63-3) moves vertically down to ‘wipe’ or ‘bend’ the part to its flanged position. In an aerial flanging process, the flanging steel moves to form the flanges in an angle rather than the vertical direction. The steel is held by the cam slide, driven by a cam driver which in turn is driven by the trim die’s downward movement. Since the finished flange forms a ‘die lock’ condition, meaning the flanged part will not be able to be lifted (retract) out of the trim die into the next die (or station), the filler cam (Figure ) is moved horizontally out of the way so the part can be lifted up and out. Once the part is removed, the filler cam moves back into its home position ready for the next drawn panel to be loaded. In the rotary cam flanging process, the filler cam is called a ‘rotor’, which rotates out of the way for the flanged part to be lifted up and out. Some parts of the rotary cam flanging design are a patented process. In comparison to the conventional cam flanging, rotary flanging has the advantage of being very compact. TYPES OF HEMMING DIES There are two types of hemming dies, as shown in Figure 63-4. Both processes have a fixed hemming bed, on which the flanged outer part is loaded; the inner panel is then loaded onto the outer panel; proper clamps are applied to hold tight the panels together and in place. In press (or table top) hemming, a pre-hemming tool is moved to form the flange into a halfway position, followed by the final hemming tool pressing down on the flange against the inner and outer panels to its final position. Many different shapes of hem tips can be achieved, as shown in the figure. In roller hemming, a pre-roller moves in a three dimensional curvilinear path following the hem tip, to form the flange partially. This is followed by a final roller, moving in another three dimensional path, to finish the hem shape. In the hemming of complex or high-end parts, many passes (rollers) are needed to achieve high quality hem surfaces. Similarly, with the design of different roller shapes, many shapes of hem tips can be achieved. APPENDIX T APPENDIX T Body-in-white part Tipping Unfold hem/flanges Detail #1 Detail #2 Unfolded part boundary Smoothed boundary P.O./Binder design Not OK OK Binder closing simulation Fill/smoothing of part boundary (3-D) Detail #2 Draw simulation Not OK OK Die structure design Addendum design/P.O. adjust Trim line Part/Product Scrap Unfold hem flange tangentially Hem flange or, unfold to flanging position Detail #1 Break line Punch opening line (Theoretical P.O. line, vertical project to the binder surface) Draw wall surface Post(punch) radius Draw wall angle Die radius Binder surface Detail #2 Figure 63-1. A typical draw die engineering process APPENDIX T 1 2 Air draw+ Toggle draw+ Air draw with pad Four-piece stretch draw++ Crash form die+ + : single action ++ : double action Figure 63-2. Types of draw dies Pad Sheet blank Post Flanging steel Pad 1 Sheet blank (initial) Post Filler cam Cam steel Cam slide Sheet blank (final) Direct flanging Cam (aerial) flanging Pad 1 Post Rotor Sheet blank (initial) Cam steel Cam slide Sheet blank (final) Rotary cam flanging Figure 63-3. Types of flanging dies APPENDIX T Final hemming tool 3D curlverlinear roller path along hem flange Inner panel Clamper Straight motions Final roller Pre-hemming tool Detail #3 Outer panel Hem bed Hem bed Pre-roller Press (or table top) hemming Roller hemming Inner panel Outer panel Detail #3 (loop hem) Figure 63-4. Types of hemming dies APPENDIX P Corporate Address Livermore Software Technology Corporation P. O. Box 712 Livermore, California 94551-0712 Support Addresses Livermore Software Technology Corporation 7374 Las Positas Road Livermore, California 94551 Tel: 925-449-2500 ♦ Fax: 925-449-2507 Email: sales@lstc.com Website: www.lstc.com Disclaimer Technology Software Livermore Corporation 1740 West Big Beaver Road Suite 100 Troy, Michigan 48084 Tel: 248-649-4728 ♦ Fax: 248-649-6328 Copyright © 1992-2019 Livermore Software Technology Corporation. All Rights Reserved. LS-DYNA®, LS-OPT® and LS-PrePost® are registered trademarks of Livermore Software Technology Corporation in the United States. All other trademarks, product names and brand names belong to their respective owners. LSTC products are protected under the following US patents: 7953578, 7945432, 7702494, 7702490, 7664623, 7660480, 7657394, 7640146, 7613585, 7590514, 7533577, 7516053, 7499050, 7472602, 7428713, 7415400, 7395128, 7392163, 7386428, 7386425, 7382367, 7308387, 7286972, 7167816, 8050897, 8069017, 7987143, 7996344, 8126684, 8150668, 8165856, 8180605, 8190408, 8200464, 8296109, 8209157, 8271237, 8200458, 8306793, Japan patent 5090426 and pending patents applications. LSTC reserves the right to modify the material contained within this manual without prior notice. The information and examples included herein are for illustrative purposes only and are not intended to be exhaustive or all-inclusive. LSTC assumes no liability or responsibility whatsoever for any direct of indirect damages or inaccuracies of any type or nature that could be deemed to have resulted from the use of this manual. Any reproduction, in whole or in part, of this manual is prohibited without the prior written approval of LSTC. All requests to reproduce the contents hereof should be sent to sales@lstc.com. AES. Copyright © 2001, Dr Brian Gladman < brg@gladman.uk.net>, Worcester, UK. All rights reserved. LICENSE TERMS The free distribution and use of this software in both source and binary form is allowed (with or without changes) provided that: 1. 2. 3. distributions of this source code include the above copyright notice, this list of conditions and the following disclaimer; distributions in binary form include the above copyright notice, this list of conditions and the following disclaimer in the documentation and/or other associated materials; the copyright holder's name is not used to endorse products built using this software without specific written permission. DISCLAIMER This software is provided 'as is' with no explicit or implied warranties in respect of any properties, This file contains the code for implementing the key schedule for AES (Rijndael) for block and key sizes of 16, 24, and 32 bytes. LS-DYNA Theory Manual Abstract 1 Abstract LS-DYNA is a general purpose finite element code for analyzing the large deformation static and dynamic response of structures including structures coupled to fluids. The main solution methodology is based on explicit time integration. An implicit solver is currently available with somewhat limited capabilities including structural analysis and heat transfer. A contact-impact algorithm allows difficult contact problems to be easily treated with heat transfer included across the contact interfaces. By a specialization of this algorithm, such interfaces can be rigidly tied to admit variable zoning without the need of mesh transition regions. Other specializa- tions, allow draw beads in metal stamping applications to be easily modeled simply by defining a line of nodes along the draw bead. Spatial discretization is achieved by the use of four node tetrahedron and eight node solid elements, two node beam elements, three and four node shell elements, eight node solid shell elements, truss elements, membrane elements, discrete elements, and rigid bodies. A variety of element formulations are available for each element type. Specialized capabilities for airbags, sensors, and seatbelts have tailored LS-DYNA for applications in the automotive industry. Adaptive remeshing is available for shell elements and is widely used in sheet metal stamping applications. LS-DYNA currently contains approximately one- hundred constitutive models and ten equations-of-state to cover a wide range of material behavior. This theoretical manual has been written to provide users and potential users with insight into the mathematical and physical basis of the code. LS-DYNA Theory Manual History of LS-DYNA 2 History of LS-DYNA The origin of LS-DYNA dates back to the public domain software, DYNA3D, which was developed in the mid-seventies at the Lawrence Livermore National Laboratory. The first version of DYNA3D [Hallquist 1976a] was released in 1976 with constant stress 4- or 8-node solid elements, 16- and 20-node solid elements with 2 × 2 × 2 Gaussian quadrature, 3, 4, and 8-node membrane elements, and a 2-node cable element. A nodal constraint contact-impact interface algorithm [Hallquist 1977] was available. On the Control Data CDC-7600, a supercomputer in 1976, the speed of the code varied from 36 minutes per 106 mesh cycles with 4-8 node solids to 180 minutes per 106 mesh cycles with 16 and 20 node solids. Without hourglass control to prevent formation of non-physical zero energy deformation modes, constant stress solids were processed at 12 minutes per 106 mesh cycles. A moderate number of very costly solutions were obtained with this version of DYNA3D using 16- and 20-node solids. Hourglass modes combined with the procedure for computing the time step size prevented us from obtaining solutions with constant stress elements. In this early development, several things became apparent. Hourglass deformation modes of the constant stress elements were invariably excited by the contact-impact algorithm, showing that a new sliding interface algorithm was needed. Higher order elements seemed to be impractical for shock wave propagation because of numerical noise resulting from the ad hoc mass lumping necessary to generate a diagonal mass matrix. Although the lower frequency structural response was accurately computed with these elements, their high computer cost made analysis so expensive as to be impractical. It was obvious that realistic three-dimensional structural calculations were possible, if and only if the under-integrated eight node constant stress solid element could be made to function. This implied a need for a much better sliding interface algorithm, a more cost-effective hourglass control, more optimal program- ming, and a machine much faster than the CDC-7600. This latter need was fulfilled several years later when LLNL took deliver of its first CRAY-1. At this time, DYNA3D was completely rewritten. History of LS-DYNA LS-DYNA Theory Manual The next version, released in 1979, achieved the aforementioned goals. On the CRAY the vectorized speed was 50 times faster, 0.67 minutes per million mesh cycles. A symmetric, penalty-based, contact-impact algorithm was considerably faster in execution speed and exceedingly reliable. Due to lack of use, the membrane and cable elements were stripped and all higher order elements were eliminated as well. Wilkins’ finite difference equations [Wilkins et al. 1974] were implemented in unvectorized form in an overlay to compare their performance with the finite element method. The finite difference algorithm proved to be nearly two times more expensive than the finite element approach (apart from vectorization) with no compensating increase in accuracy, and was removed in the next code update. The 1981 version [Hallquist 1981a] evolved from the 1979 version. Nine additional material models were added to allow a much broader range of problems to be modeled including explosive-structure and soil-structure interactions. Body force loads were implemented for angular velocities and base accelerations. A link was also established from the 3D Eulerian code JOY [Couch, et. al., 1983] for studying the structural response to impacts by penetrating projectiles. An option was provided for storing element data on disk thereby doubling the capacity of DYNA3D. The 1982 version of DYNA3D [Hallquist 1982] accepted DYNA2D [Hallquist 1980] material input directly. The new organization was such that equations of state and constitutive models of any complexity could be easily added. Complete vectorization of the material models had been nearly achieved with about a 10 percent increase in execution speed over the 1981 version. In the 1986 version of DYNA3D [Hallquist and Benson 1986], many new features were added, including beams, shells, rigid bodies, single surface contact, interface friction, discrete springs and dampers, optional hourglass treatments, optional exact volume integration, and VAX/VMS, IBM, UNIX, COS operating systems compatibility, that greatly expanded its range of applications. DYNA3D thus became the first code to have a general single surface contact algorithm. In the 1987 version of DYNA3D [Hallquist and Benson 1987] metal forming simulations and composite analysis became a reality. This version included shell thickness changes, the Belytschko-Tsay shell element [Belytschko and Tsay, 1981], and dynamic relaxation. Also included were non-reflecting boundaries, user specified integration rules for shell and beam elements, a layered composite damage model, and single point constraints. New capabilities added in the 1988 DYNA3D [Hallquist 1988] version included a cost effective resultant beam element, a truss element, a C0 triangular shell, the BCIZ triangular shell [Bazeley et al., 1965], mixing of element formulations in calculations, composite failure modeling for solids, noniterative plane stress plasticity, contact surfaces with spot welds, tiebreak sliding surfaces, beam surface contact, finite LS-DYNA Theory Manual History of LS-DYNA stonewalls, stonewall reaction forces, energy calculations for all elements, a crushable foam constitutive model, comment cards in the input, and one-dimensional slidelines. In 1988 the Hallquist began working half-time at LLNL to devote more time to the development and support of LS-DYNA for automotive applications. By the end of 1988 it was obvious that a much more concentrated effort would be required in the development of LS-DYNA if problems in crashworthiness were to be properly solved; therefore, at the start of 1989 the Hallquist resigned from LLNL to continue code development full time at Livermore Software Technology Corporation. The 1989 version introduced many enhanced capabilities including a one-way treatment of slide surfaces with voids and friction; cross-sectional forces for structural elements; an optional user specified minimum time step size for shell elements using elastic and elastoplastic material models; nodal accelerations in the time history database; a compressible Mooney-Rivlin material model; a closed-form update shell plasticity model; a general rubber material model; unique penalty specifications for each slide surface; external work tracking; optional time step criterion for 4-node shell elements; and internal element sorting to allow full vectorization of right-hand-side force assembly. 2.1 Features add in 1989-1990 Throughout the past decade, considerable progress has been made as may be seen in the chronology of the developments which follows. During 1989 many extensions and developments were completed, and in 1990 the following capabilities were delivered to users: • arbitrary node and element numbers, • fabric model for seat belts and airbags, • composite glass model, • vectorized type 3 contact and single surface contact, • many more I/O options, • all shell materials available for 8 node brick shell, • strain rate dependent plasticity for beams, • fully vectorized iterative plasticity, • interactive graphics on some computers, • nodal damping, • shell thickness taken into account in shell type 3 contact, • shell thinning accounted for in type 3 and type 4 contact, • soft stonewalls, History of LS-DYNA LS-DYNA Theory Manual • print suppression option for node and element data, • massless truss elements, rivets – based on equations of rigid body dynamics, • massless beam elements, spot welds – based on equations of rigid body dynamics, • expanded databases with more history variables and integration points, • force limited resultant beam, • rotational spring and dampers, local coordinate systems for discrete elements, • resultant plasticity for C0 triangular element, • energy dissipation calculations for stonewalls, • hourglass energy calculations for solid and shell elements, • viscous and Coulomb friction with arbitrary variation over surface, • distributed loads on beam elements, • Cowper and Symonds strain rate model, • segmented stonewalls, • stonewall Coulomb friction, • stonewall energy dissipation, • airbags (1990), • nodal rigid bodies, • automatic sorting of triangular shells into C0 groups, • mass scaling for quasi static analyses, • user defined subroutines, • warpage checks on shell elements, • thickness consideration in all contact types, • automatic orientation of contact segments, • sliding interface energy dissipation calculations, • nodal force and energy database for applied boundary conditions, • defined stonewall velocity with input energy calculations, 2.2 Options added in 1991-1992 • rigid/deformable material switching, • rigid bodies impacting rigid walls, LS-DYNA Theory Manual History of LS-DYNA • strain-rate effects in metallic honeycomb model 26, • shells and beams interfaces included for subsequent component analyses, • external work computed for prescribed displacement/velocity/accelerations, • linear constraint equations, • MPGS database, • MOVIE database, • Slideline interface file, • automated contact input for all input types, • automatic single surface contact without element orientation, • constraint technique for contact, • cut planes for resultant forces, • crushable cellular foams, • urethane foam model with hysteresis, • subcycling, • friction in the contact entities, • strains computed and written for the 8 node thick shells, • “good” 4 node tetrahedron solid element with nodal rotations, • 8 node solid element with nodal rotations, • 2 × 2 integration for the membrane element, • Belytschko-Schwer integrated beam, • thin-walled Belytschko-Schwer integrated beam, • improved LS-DYNA database control, • null material for beams to display springs and seatbelts in TAURUS, • parallel implementation on Cray and SGI computers, • coupling to rigid body codes, • seat belt capability. 2.3 Options added in 1993-1994 • Arbitrary Lagrangian Eulerian brick elements, • Belytschko-Wong-Chiang quadrilateral shell element, • Warping stiffness in the Belytschko-Tsay shell element, History of LS-DYNA LS-DYNA Theory Manual • Fast Hughes-Liu shell element, • Fully integrated brick shell element, • Discrete 3D beam element, • Generalized dampers, • Cable modeling, • Airbag reference geometry, • Multiple jet model, • Generalized joint stiffnesses, • Enhanced rigid body to rigid body contact, • Orthotropic rigid walls, • Time zero mass scaling, • Coupling with USA (Underwater Shock Analysis), • Layered spot welds with failure based on resultants or plastic strain, • Fillet welds with failure, • Butt welds with failure, • Automatic eroding contact, • Edge-to-edge contact, • Automatic mesh generation with contact entities, • Drawbead modeling, • Shells constrained inside brick elements, • NIKE3D coupling for springback, • Barlat’s anisotropic plasticity, • Superplastic forming option, • Rigid body stoppers, • Keyword input, • Adaptivity, • First MPP (Massively Parallel) version with limited capabilities. • Built in least squares fit for rubber model constitutive constants, • Large hystersis in hyperelastic foam, • Bilhku/Dubois foam model, • Generalized rubber model, LS-DYNA Theory Manual History of LS-DYNA 2.4 Version 936 New options added to version 936 in 1995 include: • Belytschko - Leviathan Shell • Automatic switching between rigid and deformable bodies. • Accuracy on SMP machines to give identical answers on one, two or more processors. • Local coordinate systems for cross-section output can now be specified. • Null material for shell elements. • Global body force loads now may be applied to a subset of materials. • User defined loading subroutine. • Improved interactive graphics. • New initial velocity options for specifying rotational velocities. • Geometry changes after dynamic relaxation can be considered for initial velocities. • Velocities may also be specified by using material or part ID’s. • Improved speed of brick element hourglass force and energy calculations. • Pressure outflow boundary conditions have been added for the ALE options. • More user control for hourglass control constants for shell elements. • Full vectorization in constitutive models for foam, models 57 and 63. • Damage mechanics plasticity model, material 81, • General linear viscoelasticity with 6 term prony series. • Least squares fit for viscoelastic material constants. • Table definitions for strain rate effects in material type 24. • Improved treatment of free flying nodes after element failure. • Automatic projection of nodes in CONTACT_TIED to eliminate gaps in the surface. • More user control over contact defaults. • Improved interpenetration warnings printed in automatic contact. • Flag for using actual shell thickness in single surface contact logic rather than the default. • Definition by exempted part ID’s. • Airbag to Airbag venting/segmented airbags are now supported. History of LS-DYNA LS-DYNA Theory Manual • Airbag reference geometry speed improvements by using the reference geometry for the time step size calculation. • Isotropic airbag material may now be directly for cost efficiency. • Airbag fabric material damping is now specified as the ratio of critical damping. • Ability to attach jets to the structure so the airbag, jets, and structure to move together. • PVM 5.1 Madymo coupling is available. • Meshes are generated within LS-DYNA3D for all standard contact entities. • Joint damping for translational motion. • Angular displacements, rates of displacements, damping forces, etc. in JNTFORC file. • Link between LS-NIKE3D to LS-DYNA3D via *INITIAL_STRESS keywords. • Trim curves for metal forming springback. • Sparse equation solver for springback. • Improved mesh generation for IGES and VDA provides a mesh that can directly be used to model tooling in metal stamping analyses. 2.5 Version 940 New options added to Version 940 in 1996 and 1997: • Part/Material ID’s may be specified with 8 digits. • Rigid body motion can be prescribed in a local system fixed to the rigid body. • Nonlinear least squares fit available for the Ogden rubber model. • Lease squares fit to the relaxation curves for the viscoelasticity in rubber. • Fu-Chang rate sensitive foam. • 6 term Prony series expansion for rate effects in model 57-now 73 • Viscoelastic material model 76 implemented for shell elements. • Mechanical threshold stress (MTS) plasticity model for rate effects. • Thermoelastic-plastic material model for Hughes-Liu beam element. • Ramberg-Osgood soil model • Invariant local coordinate systems for shell elements are optional. • Second order accurate stress updates. • Four-noded, linear, tetrahedron element. LS-DYNA Theory Manual History of LS-DYNA • Co-rotational solid element for foam that can invert without stability problems. • Improved speed in rigid body to rigid body contacts. • Improved searching for the a_3, a_5 and a10 contact types. • Invariant results on shared memory parallel machines with the a_n contact types. • Thickness offsets in type 8 and 9 tie break contact algorithms. • Bucket sort frequency can be controlled by a load curve for airbag applications. • In automatic contact each part ID in the definition may have unique: ◦ Static coefficient of friction ◦ Dynamic coefficient of friction ◦ Exponential decay coefficient ◦ Viscous friction coefficient ◦ Optional contact thickness ◦ Optional thickness scale factor ◦ Local penalty scale factor • Automatic beam-to-beam, shell edge-to-beam, shell edge-to-shell edge and single surface contact algorithm. • Release criteria may be a multiple of the shell thickness in types a_3, a_5, a10, 13, and 26 contact. • Force transducers to obtain reaction forces in automatic contact definitions. Defined manually via segments, or automatically via part ID’s. • Searching depth can be defined as a function of time. • Bucket sort frequency can be defined as a function of time. • Interior contact for solid (foam) elements to prevent "negative volumes." • Locking joint • Temperature dependent heat capacity added to Wang-Nefske inflator models. • Wang Hybrid inflator model [Wang, 1996] with jetting options and bag-to-bag venting. • Aspiration included in Wang’s hybrid model [Nucholtz, Wang, Wylie, 1996]. • Extended Wang’s hybrid inflator with a quadratic temperature variation for heat capacities [Nusholtz, 1996]. • Fabric porosity added as part of the airbag constitutive model. • Blockage of vent holes and fabric in contact with structure or itself considered in venting with leakage of gas. History of LS-DYNA LS-DYNA Theory Manual • Option to delay airbag liner with using the reference geometry until the reference area is reached. • Birth time for the reference geometry. • Multi-material Euler/ALE fluids, ◦ 2nd order accurate formulations. ◦ Automatic coupling to shell, brick, or beam elements ◦ Coupling using LS-DYNA contact options. ◦ Element with fluid + void and void material ◦ Element with multi-materials and pressure equilibrium • Nodal inertia tensors. • 2D plane stress, plane strain, rigid, and axisymmetric elements • 2D plane strain shell element • 2D axisymmetric shell element. • Full contact support in 2D, tied, sliding only, penalty and constraint techniques. • Most material types supported for 2D elements. • Interactive remeshing and graphics options available for 2D. • Subsystem definitions for energy and momentum output. and many more enhancements not mentioned above. 2.6 Version 950 Capabilities added during 1997-1998 in Version 950 include: • Adaptive refinement can be based on tooling curvature with FORMING contact. • The display of draw beads is now possible since the draw bead data is output into the d3plot database. • An adaptive box option, *DEFINE_BOX_ADAPTIVE, allows control over the refinement level and location of elements to be adapted. • A root identification file, adapt.rid, gives the parent element ID for adapted elements. • Draw bead box option, *DEFINE_BOX_DRAWBEAD, simplifies draw bead input. • The new control option, CONTROL_IMPLICIT, activates an implicit solution scheme. • 2D Arbitrary-Lagrangian-Eulerian elements. LS-DYNA Theory Manual History of LS-DYNA • 2D automatic contact is defined by listing part ID's. • 2D r-adaptivity for plane strain and axisymmetric forging simulations is available. • 2D automatic non-interactive rezoning as in LS-DYNA2D. • 2D plane strain and axisymmetric element with 2 × 2 selective-reduced integration are implemented. • Implicit 2D solid and plane strain elements are available. • Implicit 2D contact is available. • The new keyword, *DELETE_CONTACT_2DAUTO, allows the deletion of 2D automatic contact definitions. • The keyword, *LOAD_BEAM is added for pressure boundary conditions on 2D elements. • A viscoplastic strain rate option is available for materials: ◦ *MAT_PLASTIC_KINEMATIC ◦ *MAT_JOHNSON_COOK ◦ *MAT_POWER_LAW_PLASTICITY ◦ *MAT_STRAIN_RATE_DEPENDENT_PLASTICITY ◦ *MAT_PIECEWISE_LINEAR_PLASTICITY ◦ *MAT_RATE_SENSITIVE_POWERLAW_PLASTICITY ◦ *MAT_ZERILLI-ARMSTRONG ◦ *MAT_PLASTICITY_WITH_DAMAGE ◦ *MAT_PLASTICITY_COMPRESSION_TENSION • Material model, *MAT_PLASTICITY_WITH_DAMAGE, has a piecewise linear damage curve given by a load curve ID. • The Arruda-Boyce hyper-viscoelastic rubber model is available, see *MAT_AR- RUDA_BOYCE. • Transverse-anisotropic-viscoelastic material for heart tissue, see *MAT_HEART_- TISSUE. • Lung hyper-viscoelastic material, see *MAT_LUNG_TISSUE. • Compression/tension plasticity model, see *MAT_PLASTICITY_COMPRES- SION_TENSION. • The Lund strain rate model, *MAT_STEINBERG_LUND, is added to Steinberg- Guinan plasticity model. • Rate sensitive foam model, *MAT_FU_CHANG_FOAM, has been extended to include engineering strain rates, etc. History of LS-DYNA LS-DYNA Theory Manual • Model, *MAT_MODIFIED_PIECEWISE_LINEAR_PLASTICITY, is added for modeling the failure of aluminum. • Material model, *MAT_SPECIAL_ORTHOTROPIC, added for television shadow mask problems. • Erosion strain is implemented for material type, *MAT_BAMMAN_DAMAGE. • The equation of state, *EOS_JWLB, is available for modeling the expansion of explosive gases. • The reference geometry option is extended for foam and rubber materials and can be used for stress initialization, see *INITIAL_FOAM_REFERENCE_GEOM- ETRY. • A vehicle positioning option is available for setting the initial orientation and velocities, see *INITIAL_VEHICLE_KINEMATICS. • A boundary element method is available for incompressible fluid dynamics problems. • The thermal materials work with instantaneous coefficients of thermal expan- sion: ◦ *MAT_ELASTIC_PLASTIC_THERMAL ◦ *MAT_ORTHOTROPIC_THERMAL ◦ *MAT_TEMPERATURE_DEPENDENT_ORTHOTROPIC ◦ *MAT_ELASTIC_WITH_VISCOSITY. • Airbag interaction flow rate versus pressure differences. • Contact segment search option, [bricks first optional] • A through thickness Gauss integration rule with 1-10 points is available for shell elements. Previously, 5 were available. • Shell element formulations can be changed in a full deck restart. • The tied interface which is based on constraint equations, TIED_SURFACE_TO_- SURFACE, can now fail with FAILURE option. • A general failure criteria for solid elements is independent of the material type, see *MAT_ADD_EROSION • Load curve control can be based on thinning and a flow limit diagram, see *DE- FINE_CURVE_FEEDBACK. • An option to filter the spotweld resultant forces prior to checking for failure has been added the option, *CONSTRAINED_SPOTWELD, by appending,_FIL- TERED_FORCE, to the keyword. • Bulk viscosity is available for shell types 1, 2, 10, and 16. LS-DYNA Theory Manual History of LS-DYNA • When defining the local coordinate system for the rigid body inertia tensor a local coordinate system ID can be used. This simplifies dummy positioning. • Prescribing displacements, velocities, and accelerations is now possible for rigid body nodes. • One-way flow is optional for segmented airbag interactions. • Pressure time history input for airbag type, LINEAR_FLUID, can be used. • An option is available to independently scale system damping by part ID in each of the global directions. • An option is available to independently scale global system damping in each of the global directions. • Added option to constrain global DOF along lines parallel with the global axes. The keyword is *CONSTRAINED_GLOBAL. This option is useful for adaptive remeshing. • Beam end code releases are available, see *ELEMENT_BEAM. • An initial force can be directly defined for the cable material, *MAT_CABLE_- DISCRETE_BEAM. The specification of slack is not required if this option is used. • Airbag pop pressure can be activated by accelerometers. • Termination may now be controlled by contact, via *TERMINATION_CON- TACT. • Modified shell elements types 8, 10 and the warping stiffness option in the Belytschko-Tsay shell to ensure orthogonality with rigid body motions in the event that the shell is badly warped. This is optional in the Belytschko-Tsay shell and the type 10 shell. • A one point quadrature brick element with an exact hourglass stiffness matrix has been implemented for implicit and explicit calculations. • Automatic file length determination for d3plot binary database is now imple- mented. This insures that at least a single state is contained in each d3plot file and eliminates the problem with the states being split between files. • The dump files, which can be very large, can be placed in another directory by specifying d=/home/user /test/d3dump on the execution line. • A print flag controls the output of data into the MATSUM and RBDOUT files by part ID's. The option, PRINT, has been added as an option to the *PART key- word. • Flag has been added to delete material data from the d3thdt file. See *DATA- BASE_EXTENT_BINARY and column 25 of the 19th control card in the struc- tured input. History of LS-DYNA LS-DYNA Theory Manual • After dynamic relaxation completes, a file is written giving the displaced state which can be used for stress initialization in later runs. 2.7 Version 960 Capabilities added during 1998-2000 in Version 960. Most new capabilities work on both the MPP and SMP versions; however, the capabilities that are implemented for the SMP version only, which were not considered critical for this release, are flagged below. These SMP unique capabilities are being extended for MPP calculations and will be available in the near future. The implicit capabilities for MPP require the development of a scalable eigenvalue solver, which is under development for a later release of LS- DYNA. • Incompressible flow solver is available. Structural coupling is not yet imple- mented. • Adaptive mesh coarsening can be done before the implicit spring back calcula- tion in metal forming applications. • Two-dimensional adaptivity can be activated in both implicit and explicit calculations. (SMP version only) • An internally generated smooth load curve for metal forming tool motion can be activated with the keyword: *DEFINE_CURVE_SMOOTH. • Torsional forces can be carried through the deformable spot welds by using the contact type: *CONTACT_SPOTWELD_WITH_TORSION (SMP version only with a high priority for the MPP version if this option proves to be stable.) • Tie break automatic contact is now available via the *CONTACT_AUTOMAT- IC_..._TIEBREAK options. This option can be used for glued panels. (SMP only) • *CONTACT_RIGID_SURFACE option is now available for modeling road surfaces (SMP version only). • Fixed rigid walls PLANAR and PLANAR_FINITE are represented in the binary output file by a single shell element. • Interference fits can be modeled with the INTERFERENCE option in contact. • A layered shell theory is implemented for several constitutive models including the composite models to more accurately represent the shear stiffness of laminat- ed shells. • Damage mechanics is available to smooth the post-failure reduction of the resultant forces in the constitutive model *MAT_SPOTWELD_DAMAGE. • Finite elastic strain isotropic plasticity model is available for solid elements. *MAT_FINITE_ELASTIC_STRAIN_PLASTICITY. • A shape memory alloy material is available: *MAT_SHAPE_MEMORY. LS-DYNA Theory Manual History of LS-DYNA • Reference geometry for material, *MAT_MODIFIED_HONEYCOMB, can be set at arbitrary relative volumes or when the time step size reaches a limiting value. This option is now available for all element types including the fully integrated solid element. • Non orthogonal material axes are available in the airbag fabric model. See *MAT_FABRIC. • Other new constitutive models include for the beam elements: ◦ *MAT_MODIFIED_FORCE_LIMITED ◦ *MAT_SEISMIC_BEAM ◦ *MAT_CONCRETE_BEAM • for shell and solid elements: ◦ *MAT_ELASTIC_VISCOPLASTIC_THERMAL • for the shell elements: ◦ *MAT_GURSON ◦ *MAT_GEPLASTIC_SRATE2000 ◦ *MAT_ELASTIC_VISCOPLASTIC_THERMAL ◦ *MAT_COMPOSITE_LAYUP ◦ *MAT_COMPOSITE_LAYUP ◦ *MAT_COMPOSITE_direct • for the solid elements: ◦ *MAT_JOHNSON_HOLMQUIST_CERAMICS ◦ *MAT_JOHNSON_HOLMQUIST_CONCRETE ◦ *MAT_INV_HYPERBOLIC_SIN ◦ *MAT_UNIFIED_CREEP ◦ *MAT_SOIL_BRICK ◦ *MAT_DRUCKER_PRAGER ◦ *MAT_RC_SHEAR_WALL • and for all element options a very fast and efficient version of the Johnson-Cook plasticity model is available: ◦ *MAT_SIMPLIFIED_JOHNSON_COOK • A fully integrated version of the type 16 shell element is available for the resultant constitutive models. History of LS-DYNA LS-DYNA Theory Manual • A nonlocal failure theory is implemented for predicting failure in metallic materials. The keyword *MAT_NONLOCAL activates this option for a subset of elastoplastic constitutive models. • A discrete Kirchhoff triangular shell element (DKT) for explicit analysis with three in plane integration points is flagged as a type 17 shell element. This element has much better bending behavior than the C0 triangular element. • A discrete Kirchhoff linear triangular and quadrilaterial shell element is available as a type 18 shell. This shell is for extracting normal modes and static analysis. • A C0 linear 4-node quadrilaterial shell element is implemented as element type 20 with drilling stiffness for normal modes and static analysis. • An assumed strain linear brick element is available for normal modes and statics. • The fully integrated thick shell element has been extended for use in implicit calculations. • A fully integrated thick shell element based on an assumed strain formulation is now available. This element uses a full 3D constitutive model which includes the normal stress component and, therefore, does not use the plane stress assump- tion. • The 4-node constant strain tetrahedron element has been extended for use in implicit calculations. • Relative damping between parts is available, see *DAMPING_RELATIVE (SMP only). • Preload forces are can be input for the discrete beam elements. • Objective stress updates are implemented for the fully integrated brick shell element. • Acceleration time histories can be prescribed for rigid bodies. • Prescribed motion for nodal rigid bodies is now possible. • Generalized set definitions, i.e., SET_SHELL_GENERAL etc. provide much flexibility in the set definitions. • The command "sw4." will write a state into the dynamic relaxation file, D3DRLF, during the dynamic relaxation phase if the d3drlf file is requested in the input. • Added mass by PART ID is written into the matsum file when mass scaling is used to maintain the time step size, (SMP version only). • Upon termination due to a large mass increase during a mass scaled calculation a print summary of 20 nodes with the maximum added mass is printed. • Eigenvalue analysis of models containing rigid bodies is now available using BCSLIB-EXT solvers from Boeing. (SMP version only). LS-DYNA Theory Manual History of LS-DYNA • Second order stress updates can be activated by part ID instead of globally on the *CONTROL_ACCURACY input. • Interface frictional energy is optionally computed for heat generation and is output into the interface force file (SMP version only). • The interface force binary database now includes the distance from the contact surface for the FORMING contact options. This distance is given after the nodes are detected as possible contact candidates. (SMP version only). • Type 14 acoustic brick element is implemented. This element is a fully integrated version of type 8, the acoustic element (SMP version only). • A flooded surface option for acoustic applications is available (SMP version only). • Attachment nodes can be defined for rigid bodies. This option is useful for NVH applications. • CONSTRAINED_POINTS tie any two points together. These points must lie on a shell element. • Soft constraint is available for edge-to-edge contact in type 26 contact. • CONSTAINED_INTERPOLATION option for beam to solid interfaces and for spreading the mass and loads. (SMP version only). • A database option has been added that allows the output of added mass for shell elements instead of the time step size. • A new contact option allows the inclusion of all internal shell edges in contact type *CONTACT_GENERAL, type 26. This option is activated by adding INTE- RIOR option. • A new option allows the use deviatoric strain rates rather than total rates in material model 24 for the Cowper-Symonds rate model. • The CADFEM option for ASCII databases is now the default. Their option includes more significant figures in the output files. • When using deformable spot welds, the added mass for spot welds is now printed for the case where global mass scaling is activated. This output is in the log file, d3hsp file, and the messag file. • Initial penetration warnings for edge-to-edge contact are now written into the MESSAG file and the D3HSP file. • Each compilation of LS-DYNA is given a unique version number. • Finite length discrete beams with various local axes options are now available for material types 66, 67, 68, 93, and 95. In this implementation the absolute value of SCOOR must be set to 2 or 3 in the *SECTION_BEAM input. • New discrete element constitutive models are available: History of LS-DYNA LS-DYNA Theory Manual ◦ *MAT_ELASTIC_SPRING_DISCRETE_BEAM ◦ *MAT_INELASTIC_SPRING_DISCRETE_BEAM ◦ *MAT_ELASTIC_6DOF_SPRING_DISCRETE_BEAM ◦ *MAT_INELASTIC_6DOF_SPRING_DISCRETE_BEAM The latter two can be used as finite length beams with local coordinate systems. • Moving SPC's are optional in that the constraints are applied in a local system that rotates with the 3 defining nodes. • A moving local coordinate system, CID, can be used to determine orientation of discrete beam elements. • Modal superposition analysis can be performed after an eigenvalue analysis. Stress recovery is based on type 18 shell and brick (SMP only). • Rayleigh damping input factor is now input as a fraction of critical damping, i.e. 0.10. The old method required the frequency of interest and could be highly unstable for large input values. • Airbag option "SIMPLE_PRESSURE_VOLUME" allows for the constant CN to be replaced by a load curve for initialization. Also, another load curve can be defined which allows CN to vary as a function of time during dynamic relaxa- tion. After dynamic relaxation CN can be used as a fixed constant or load curve. • Hybrid inflator model utilizing CHEMKIN and NIST databases is now available. Up to ten gases can be mixed. • Option to track initial penetrations has been added in the automatic SMP contact types rather than moving the nodes back to the surface. This option has been available in the MPP contact for some time. This input can be defined on the fourth card of the *CONTROL_CONTACT input and on each contact definition on the third optional card in the *CONTACT definitions. • If the average acceleration flag is active, the average acceleration for rigid body nodes is now written into the d3thdt and nodout files. In previous versions of LS-DYNA, the accelerations on rigid nodes were not averaged. • A capability to initialize the thickness and plastic strain in the crash model is available through the option *INCLUDE_STAMPED_PART, which takes the results from the LS-DYNA stamping simulation and maps the thickness and strain distribution onto the same part with a different mesh pattern. • A capability to include finite element data from other models is available through the option, *INCLUDE_TRANSFORM. This option will take the model defined in an INCLUDE file: offset all ID's; translate, rotate, and scale the coordi- nates; and transform the constitutive constants to another set of units. LS-DYNA Theory Manual History of LS-DYNA 2.8 Version 970 Many new capabilities were added during 2001-2002 to create version 970 of LS-DYNA. Some of the new features, which are also listed below, were also added to later releases of version 960. Most new explicit capabilities work for both the MPP and SMP versions; however, the implicit capabilities for MPP require the development of a scalable eigenvalue solver and a parallel implementation of the constraint equations into the global matrices. This work is underway. A later release of version 970 is planned that will be scalable for implicit solutions. • MPP decomposition can be controlled using *CONTROL_MPP_DECOMPOSI- TION commands in the input deck. • The MPP arbitrary Lagrangian-Eulerian fluid capability now works for airbag deployment in both SMP and MPP calculations. • Euler-to-Euler coupling is now available through the keyword *CON- STRAINED_EULER_TO_EULER. • Up to ten ALE multi-material groups may now be defined. The previous limit was three groups. • Volume fractions can be automatically assigned during initialization of multi- material cells. See the GEOMETRY option of *INITIAL_VOLUME_FRACTION. • A new ALE smoothing option is available to accurately predict shock fronts. • DATABASE_FSI activates output of fluid-structure interaction data to ASCII file DBFSI. • Point sources for airbag inflators are available. The origin and mass flow vector of these inflators are permitted to vary with time. • A majority of the material models for solid materials are available for calcula- tions using the SPH (Smooth Particle Hydrodynamics) option. • The Element Free Galerkin method (EFG or meshfree) is available for two- dimensional and three-dimensional solids. This new capability is not yet imple- mented for MPP applications. • A binary option for the ASCII files is now available. This option applies to all ASCII files and results in one binary file that contains all the information normal- ly spread between a large number of separate ASCII files. • Material models can now be defined by numbers rather than long names in the keyword input. For example the keyword *MAT_PIECEWISE_LINEAR_PLAS- TICITY can be replaced by the keyword: *MAT_024. • An embedded NASTRAN reader for direct reading of NASTRAN input files is available. This option allows a typical input file for NASTRAN to be read direct- ly and used without additional input. See the *INCLUDE_NASTRAN keyword. History of LS-DYNA LS-DYNA Theory Manual • Names in the keyword input can represent numbers if the *PARAMETER option is used to relate the names and the corresponding numbers. • Model documentation for the major ASCII output files is now optional. This option allows descriptors to be included within the ASCII files that document the contents of the file. • ID’s have been added to the following keywords: ◦ *BOUNDARY_PRESCRIBED_MOTION ◦ *BOUNDARY_PRESCRIBED_SPC ◦ *CONSTRAINED_GENERALIZED_WELD ◦ *CONSTRAINED_JOINT ◦ *CONSTRAINED_NODE_SET ◦ *CONSTRAINED_RIVET ◦ *CONSTRAINED_SPOTWELD ◦ *DATABASE_CROSS_SECTION ◦ *ELEMENT_MASS • The *DATABASE_ADAMS keyword is available to output a modal neutral file d3mnf. This is available upon customer request since it requires linking to an ADAMS library file. • Penetration warnings for the contact option, “ignore initial penetration,” are added as an option. Previously, no penetration warnings were written when this contact option was activated. • Penetration warnings for nodes in-plane with shell mid-surface are printed for the AUTOMATIC contact options. Previously, these nodes were ignored since it was assumed that they belonged to a tied interface where an offset was not used; consequently, they should not be treated in contact. • For the arbitrary spot weld option, the spot welded nodes and their contact segments are optionally written into the d3hsp file. See *CONTROL_CON- TACT. • For the arbitrary spot weld option, if a segment cannot be found for the spot welded node, an option now exists to error terminate. See *CONTROL_CON- TACT. • Spot weld resultant forces are written into the swforc file for solid elements used as spot welds. • Solid materials have now been added to the failed element report and additional information is written for the “node is deleted” messages. • A new option for terminating a calculation is available, *TERMINATION_- CURVE. LS-DYNA Theory Manual History of LS-DYNA • A 10-noded tetrahedron solid element is available with either a 4 or 5 point integration rule. This element can also be used for implicit solutions. • A new 4 node linear shell element is available that is based on Wilson’s plate element combined with a Pian-Sumihara membrane element. This is shell type 21. • A shear panel element has been added for linear applications. This is shell type 22. This element can also be used for implicit solutions. • A null beam element for visualization is available. The keyword to define this null beam is *ELEMENT_PLOTEL. This element is necessary for compatibility with NASTRAN. • A scalar node can be defined for spring-mass systems. The keyword to define this node is *NODE_SCALAR. This node can have from 1 to 6 scalar degrees-of- freedom. • A thermal shell has been added for through-thickness heat conduction. Internally, 8 additional nodes are created, four above and four below the mid- surface of the shell element. A quadratic temperature field is modeled through the shell thickness. Internally, the thermal shell is a 12 node solid element. • A beam OFFSET option is available for the *ELEMENT_BEAM definition to permit the beam to be offset from its defining nodal points. This has the ad- vantage that all beam formulations can now be used as shell stiffeners. • A beam ORIENTATION option for orienting the beams by a vector instead of the third node is available in the *ELEMENT_BEAM definition for NASTRAN compatibility. • Non-structural mass has been added to beam elements for modeling trim mass and for NASTRAN compatibility. • An optional checking of shell elements to avoid abnormal terminations is available. See *CONTROL_SHELL. If this option is active, every shell is checked each time step to see if the distortion is so large that the element will invert, which will result in an abnormal termination. If a bad shell is detected, either the shell will be deleted or the calculation will terminate. The latter is controlled by the input. • An offset option is added to the inertia definition. See *ELEMENT_INERTIA_- OFFSET keyword. This allows the inertia tensor to be offset from the nodal point. • Plastic strain and thickness initialization is added to the draw bead contact option. See *CONTACT_DRAWBEAD_INITIALIZE. • Tied contact with offsets based on both constraint equations and beam elements for solid elements and shell elements that have 3 and 6 degrees-of-freedom per node, respectively. See BEAM_OFFSET and CONSTRAINED_OFFSET contact options. These options will not cause problems for rigid body motions. History of LS-DYNA LS-DYNA Theory Manual • The segment-based (SOFT = 2) contact is implemented for MPP calculations. This enables airbags to be easily deployed on the MPP version. • Improvements are made to segment-based contact for edge-to-edge and sliding conditions, and for contact conditions involving warped segments. • An improved interior contact has been implemented to handle large shear deformations in the solid elements. A special interior contact algorithm is avail- able for tetrahedron elements. • Coupling with MADYMO 6.0 uses an extended coupling that allows users to link most MADYMO geometric entities with LS-DYNA FEM simulations. In this coupling MADYMO contact algorithms are used to calculate interface forces between the two models. • Release flags for degrees-of-freedom for nodal points within nodal rigid bodies are available. This makes the nodal rigid body option nearly compatible with the RBE2 option in NASTRAN. • Fast updates of rigid bodies for metal forming applications can now be accomplished by ignoring the rotational degrees-of-freedom in the rigid bodies that are typically inactive during sheet metal stamping simulations. See the keyword: *CONTROL_RIGID. • Center of mass constraints can be imposed on nodal rigid bodies with the SPC option in either a local or a global coordinate system. • Joint failure based on resultant forces and moments can now be used to simulate the failure of joints. • CONSTRAINED_JOINT_STIFFNESS now has a TRANSLATIONAL option for the translational and cylindrical joints. • Joint friction has been added using table look-up so that the frictional moment can now be a function of the resultant translational force. • The nodal constraint options *CONSTRAINED_INTERPOLATION and *CON- STRAINED_LINEAR now have a local option to allow these constraints to be applied in a local coordinate system. • Mesh coarsening can now be applied to automotive crash models at the beginning of an analysis to reduce computation times. See the new keyword: *CONTROL_COARSEN. • Force versus time seatbelt pretensioner option has been added. • Both static and dynamic coefficients of friction are available for seat belt slip rings. Previously, only one friction constant could be defined. • *MAT_SPOTWELD now includes a new failure model with rate effects as well as additional failure options. • Constitutive models added for the discrete beam elements: LS-DYNA Theory Manual History of LS-DYNA ◦ *MAT_1DOF_GENERALIZED_SPRING ◦ *MAT_GENERAL_NONLINEAR_6dof_DISCRETE_BEAM ◦ *MAT_GENERAL_NONLINEAR_1dof_DISCRETE_BEAM ◦ *MAT_GENERAL_SPRING_DISCRETE_BEAM ◦ *MAT_GENERAL_JOINT_DISCRETE_BEAM ◦ *MAT_SEISMIC_ISOLATOR • for shell and solid elements: ◦ *MAT_PLASTICITY_WITH_DAMAGE_ORTHO ◦ *MAT_SIMPLIFIED_JOHNSON_COOK_ORTHOTROPIC_DAMAGE ◦ *MAT_HILL_3R ◦ *MAT_GURSON_RCDC • for the solid elements: ◦ *MAT_SPOTWELD ◦ *MAT_HILL_FOAM ◦ *MAT_WOOD ◦ *MAT_VISCOELASTIC_HILL_FOAM ◦ *MAT_LOW_DENSITY_SYNTHETIC_FOAM ◦ *MAT_RATE_SENSITIVE_POLYMER ◦ *MAT_QUASILINEAR VISCOELASTIC ◦ *MAT_TRANSVERSELY_ANISOTROPIC_CRUSHABLE_FOAM ◦ *MAT_VACUUM ◦ *MAT_MODIFIED_CRUSHABLE_FOAM ◦ *MAT_PITZER_CRUSHABLE FOAM ◦ *MAT_JOINTED_ROCK ◦ *MAT_SIMPLIFIED_RUBBER ◦ *MAT_FHWA_SOIL ◦ *MAT_SCHWER_MURRAY_CAP_MODEL • Failure time added to MAT_EROSION for solid elements. • Damping in the material models *MAT_LOW_DENSITY_FOAM and *MAT_- LOW_DENSITY_VISCOUS_FOAM can now be a tabulated function of the smallest stretch ratio. • The material model *MAT_PLASTICITY_WITH_DAMAGE allows the table definitions for strain rate. History of LS-DYNA LS-DYNA Theory Manual • Improvements in the option *INCLUDE_STAMPED_PART now allow all history data to be mapped to the crash part from the stamped part. Also, symmetry planes can be used to allow the use of a single stamping to initialize symmetric parts. • Extensive improvements in trimming result in much better elements after the trimming is completed. Also, trimming can be defined in either a local or global coordinate system. This is a new option in *DEFINE_CURVE_TRIM. • An option to move parts close before solving the contact problem is available, see *CONTACT_AUTO_MOVE. • An option to add or remove discrete beams during a calculation is available with the new keyword: *PART_SENSOR. • Multiple jetting is now available for the Hybrid and Chemkin airbag inflator models. • Nearly all constraint types are now handled for implicit solutions. • Calculation of constraint and attachment modes can be easily done by using the option: *CONTROL_IMPLICIT_MODES. • Penalty option, see *CONTROL_CONTACT, now applies to all *RIGIDWALL options and is always used when solving implicit problems. • Solid elements types 3 and 4, the 4 and 8 node elements with 6 degrees-of- freedom per node, are available for implicit solutions. • The warping stiffness option for the Belytschko-Tsay shell is implemented for implicit solutions. The Belytschko-Wong-Chang shell element is now available for implicit applications. The full projection method is implemented due to it accuracy over the drill projection. • Rigid to deformable switching is implemented for implicit solutions. • Automatic switching can be used to switch between implicit and explicit calculations. See the keyword: *CONTROL_IMPLICIT_GENERAL. • Implicit dynamics rigid bodies are now implemented. See the keyword *CON- TROL_IMPLICIT_DYNAMIC. • Eigenvalue solutions can be intermittently calculated during a transient analysis. • A linear buckling option is implemented. See the new control input: *CON- TROL_IMPLICIT_BUCKLE • Implicit initialization can be used instead of dynamic relaxation. See the keyword *CONTROL_DYNAMIC_RELAXATION where the parameter, IDFLG, is set to 5. • Superelements, i.e., *ELEMENT_DIRECT_MATRIX_INPUT, are now available for implicit applications. LS-DYNA Theory Manual History of LS-DYNA • There is an extension of the option, *BOUNDARY_CYCLIC, to symmetry planes in the global Cartesian system. Also, automatic sorting of nodes on symmetry planes is now done by LS-DYNA. • Modeling of wheel-rail contact for railway applications is now available, see *RAIL_TRACK and *RAIL_TRAIN. • A new, reduced CPU, element formulation is available for vibration studies when elements are aligned with the global coordinate system. See *SECTION_- SOLID and *SECTION_SHELL formulation 98. • An option to provide approximately constant damping over a range of frequen- cies is implemented, see *DAMPING_FREQUENCY_RANGE. LS-DYNA Theory Manual Preliminaries 3 Preliminaries NOTE: Einstein summation convention is used. For each re- peated index there is an implied summation. Consider the body shown in Figure 3.1. We are interested in time-dependent deformation for which a point in b initially at 𝑋𝛼 (𝛼 = 1, 2, 3) in a fixed rectangular Cartesian coordinate system moves to a point 𝑥𝑖 (𝑖 = 1, 2, 3) in the same coordinate system. Since a Lagrangian formulation is considered, the deformation can be expressed in terms of the convected coordinates 𝑋𝛼, and time 𝑡 At time 𝑡 = 0, we have the initial conditions 𝑥𝑖 = 𝑥𝑖(𝑋𝛼, 𝑡). 𝑥𝑖(𝐗, 0) = 𝑋i 𝑥̇𝑖(𝐗, 0) = 𝑉𝑖(𝐗) where 𝐕 is the initial velocity. 3.1 Governing Equations We seek a solution to the momentum equation 𝜎𝑖𝑗,𝑗 + 𝜌𝑓𝑖 = 𝜌𝑥̈𝑖 satisfying the traction boundary conditions, 𝜎𝑖𝑗𝑛𝑗 = 𝑡𝑖(𝑡), on boundary 𝜕𝑏1, the displacement boundary conditions, 𝑥𝑖(𝑋𝛼, 𝑡) = 𝐷𝑖(𝑡), on boundary 𝜕𝑏2, and the contact discontinuity condition, (𝜎𝑖𝑗 + − 𝜎𝑖𝑗 −)𝑛𝑖 = 0, (3.1) (3.2) (3.3) (3.4) (3.5) (3.6) Preliminaries LS-DYNA Theory Manual + = 𝑥𝑖 −. Here 𝛔 is the Cauchy stress, 𝜌 is the along an interior boundary 𝜕b3 when 𝑥𝑖 current density, 𝐟 is the body force density, and 𝐱̈ is acceleration. The comma on 𝜎𝑖𝑗,𝑗 denotes covariant differentiation, and 𝑛𝑗 is a unit outward normal to a boundary element on ∂b. Mass conservation is trivially stated as where 𝑉 is the relative volume, i.e., the determinant of the deformation gradient matrix, 𝐹𝑖𝑗, 𝜌𝑉 = 𝜌0 (3.7) 𝐹𝑖𝑗 = ∂𝑥𝑖 ∂𝑋𝑗 and 𝜌0 is the reference density. The energy equation 𝐸̇ = 𝑉𝑠𝑖𝑗𝜀̇𝑖𝑗 − (𝑝 + 𝑞)𝑉̇ (3.8) (3.9) is integrated in time and is used for evaluating equations of state and to track the global energy balance. In Equation (3.9), 𝑠𝑖𝑗 and 𝑝 represent the deviatoric stresses and pressure, 𝑠𝑖𝑗 = 𝜎𝑖𝑗 + (𝑝 + 𝑞)𝛿𝑖𝑗 𝑝 = − = − 𝜎𝑖𝑗𝛿𝑖𝑗 − 𝑞 𝜎𝑘𝑘 − 𝑞 (3.10) (3.11) respectively, where 𝑞 is the bulk viscosity, 𝛿𝑖𝑗 is the Kronecker delta (𝛿𝑖𝑗 = 1 if 𝑖 = 𝑗; otherwise 𝛿𝑖𝑗 = 0), and 𝜀̇𝑖𝑗 is the strain rate tensor. The strain rates and bulk viscosity are discussed later. LS-DYNA Theory Manual Preliminaries X3 x3 x2 X2 ∂ t = 0 B0 ∂ X1 x1 Figure 3.1. Notation. We can write: ∫ (𝜌𝑥̈𝑖 − 𝜎𝑖𝑗,𝑗 − 𝜌𝑓 )𝛿𝑥𝑖𝑑𝜐 + ∫ (𝜎𝑖𝑗𝑛𝑗 − 𝑡𝑖)𝛿𝑥𝑖𝑑𝑠 𝜕𝑏1 + ∫ (𝜎𝑖𝑗 𝜕𝑏3 + − 𝜎𝑖𝑗 −)𝑛𝑗𝛿𝑥𝑖𝑑𝑠 = 0 (3.12) where 𝛿𝑥𝑖 satisfies all boundary conditions on 𝜕𝑏2, and the integrations are over the current geometry. Application of the divergence theorem gives ∫ (𝜎𝑖𝑗𝛿𝑥𝑖) ,𝑗 𝑑𝜐 = ∫ 𝜎𝑖𝑗𝑛𝑗𝛿𝑥𝑖𝑑𝑠 ∂𝑏1 and noting that + ∫ (𝜎𝑖𝑗 ∂𝑏3 + − 𝜎𝑖𝑗 −)𝑛𝑗𝛿𝑥𝑖𝑑𝑠 leads to the weak form of the equilibrium equation, (𝜎𝑖𝑗𝛿𝑥𝑖),𝑗− 𝜎𝑖𝑗,𝑗𝛿𝑥𝑖 = 𝜎𝑖𝑗𝛿𝑥𝑖,𝑗 𝛿𝜋 = ∫ 𝜌𝑥̈𝑖𝛿𝑥𝑖𝑑𝜐 + ∫ 𝜎𝑖𝑗𝛿𝑥𝑖,𝑗𝑑𝜐 − ∫ 𝜌𝑓𝑖𝛿𝑥𝑖𝑑𝜐 − ∫ 𝑡𝑖𝛿𝑥𝑖𝑑𝑠 ∂𝑏1 = 0, which is a statement of the principle of virtual work. (3.13) (3.14) (3.15) We superimpose a mesh of finite elements interconnected at nodal points on the reference configuration and track particles through time, i.e., 𝑥𝑖(𝑋𝛼, 𝑡) = 𝑥𝑖(𝑋𝛼(𝜉 , 𝜂, 𝜁 ), 𝑡) = ∑ 𝑁𝑗(𝜉 , 𝜂, 𝜁 )𝑥𝑖 𝑗(𝑡) (3.16) 𝑗=1 Preliminaries LS-DYNA Theory Manual where 𝑁𝑗 are shape (interpolation) functions in the parametric coordinates (𝜉 , 𝜂, 𝜁 ), 𝑘 is 𝑗 is the nodal coordinate of the jth the number of nodal points defining the element, and 𝑥𝑖 node in the ith direction. Each shape function has a finite support that is limited to the elements for which its associated node is a member (hence the name finite element method). Consequently, within each element the interpolation only depends on the nodal values for the nodes in that element, and hence expressions like Equation (3.16)are meaningful. The condition 𝛿𝜋 = 0 holds for all variations, 𝛿𝑥𝑖, and, in particular, it holds for variations along the shape functions. In each of the 3 Cartesian directions upon setting the variation to one of the shape functions the weak form reduces to a necessary (but not sufficient) condition that must be satisfied by any solution so that the number of equations = 3 × number of nodes. At this stage it is useful to introduce a vector space having dimension ℝ(number of nodes) number of nodes. Since the body is discretized into with a corresponding cartesian basis {𝐞𝑖 𝑛 disjoint elements, the integral in (3.15) may be separated using the spatial additively of integration into 𝑛 terms, one for each element ′}𝑖=1 𝛿𝜋 = ∑ 𝛿𝜋𝑚 = 0 . 𝑚=1 The contribution from each element is 𝛿𝜋𝑚 = ∫ 𝜌𝑥̈𝑖𝛿𝑥𝑖𝑑𝜐 𝜐𝑚 + ∫ 𝜎𝑖𝑗𝛿𝑥𝑖,𝑗𝑑𝜐 𝜐𝑚 − ∫ 𝜌𝑓𝑖𝛿𝑥𝑖𝑑𝜐 𝜐𝑚 − ∫ ∂𝑏1∩𝜕𝑣𝑚 𝑡𝑖𝛿𝑥𝑖𝑑𝑠 . Assembling the element contributions back into a system of equations leads to ∑ {∫ 𝜌𝑥̈𝑖(𝐞i⨂𝛎𝑚)𝑑𝜐 + 𝑚=1 𝜐𝑚 𝑚(𝐞i⨂𝛎,𝑗 𝑚)𝑑𝜐 ∫ 𝜎𝑖𝑗 𝜐𝑚 − ∫ 𝜌𝑓𝑖(𝐞i⨂𝛎𝑚)𝑑𝜐 𝜐𝑚 − ∫ ∂𝑏1∩𝜕𝑣𝑚 𝑡𝑖(𝐞i⨂𝛎𝑚)𝑑𝑠 } = 0. In which 𝛎𝑚 = ∑ 𝑁𝑖𝐞𝑛𝑚(𝑖) ′ (3.17) (3.18) (3.19) (3.20) where 𝑛𝑚(𝑖) is the global node number. 𝑖=1 Applying the approximation scheme of Equation (3.16) to the dependent variables and substituting into Equation (3.19) yields ∑ {∫ 𝜌𝐍𝑚 𝜐𝑚 𝑚=1 T 𝐍𝑚𝐚𝑑𝜐 + ∫ 𝐁𝑚 𝜐𝑚 T 𝛔𝑑𝜐 − ∫ 𝜌𝐍𝑚 𝜐𝑚 T 𝐛𝑑𝜐 − ∫ 𝐍𝑚 ∂𝑏1 T 𝐭𝑑𝑠 } = 0 where 𝐍 is an interpolation matrix; 𝜎 is the stress vector 𝛔T = (𝜎𝑥𝑥, 𝜎𝑦𝑦, 𝜎𝑧𝑧, 𝜎𝑥𝑦, 𝜎𝑦𝑧, 𝜎zx); (3.21) (3.22) LS-DYNA Theory Manual Preliminaries B is the strain-displacement matrix; a is the nodal acceleration vector 𝑥̈1 ⎤ = 𝐍 ⎡ 𝑥̈2 ⎥ ⎢ 𝑥̈3⎦ ⎣ 𝑎𝑥 ⎤ ⎡ ⎥ ⎢ 𝑎𝑥 ⎥ ⎢ ⋮ ⎥ ⎢ ⎥ ⎢ 𝑎𝑦 ⎥ ⎢ 𝑘⎦ 𝑎𝑧 ⎣ = 𝐍𝐚; (3.23) b is the body force load vector; and 𝒕 is the applied traction load. 𝐛 = 𝑓𝑥 ⎤ ⎡ 𝑓𝑦 ⎥⎥ ⎢⎢ 𝑓𝑧⎦ ⎣ , 𝐭 = 𝑡𝑥 ⎤ ⎡ 𝑡𝑦 ⎥ ⎢ 𝑡𝑧⎦ ⎣ (3.24) LS-DYNA Theory Manual Solid Elements 4 Solid Elements For a mesh of 8-node hexahedron solid elements, Equation ((3.16)) becomes: 𝑥𝑖(𝑋𝛼, 𝑡) = 𝑥𝑖(𝑋𝛼(𝜉 , 𝜂, 𝜁 ), 𝑡) = ∑ 𝜙𝑗(𝜉 , 𝜂, 𝜁 )𝑥𝑖 𝑗(𝑡) . The shape function 𝜙𝑗 is defined for the 8-node hexahedron as 𝑗=1 𝜙𝑗 = (1 + 𝜉 𝜉𝑗)(1 + 𝜂𝜂𝑗)(1 + 𝜁 𝜁𝑗), (4.1) (4.2) where 𝜉𝑗, 𝜂𝑗, 𝜁𝑗 take on their nodal values of (±1, ±1, ±1) and 𝑥𝑖 the jth node in the ith direction . 𝑗 is the nodal coordinate of For a solid element, N is the 3 × 24 rectangular interpolation matrix given by N(𝜉 , 𝜂, 𝜁 ) = 𝜙1 ⎡ ⎢ ⎣ 𝜙1 𝜙1 𝜙2 0 ⋯ 0 𝜙2 ⋯ 𝜙8 0 ⋯ 0 ⎤ , ⎥ 𝜙8⎦ 𝝈 is the stress vector σT = (𝜎𝑥𝑥 𝜎𝑦𝑦 𝜎𝑧𝑧 𝜎𝑥𝑦 𝜎𝑦𝑧 𝜎𝑧𝑥). (4.3) (4.4) Solid Elements LS-DYNA Theory Manual Node -1 -1 -1 -1 -1 -1 -1 -1 -1 -1 -1 -1 Figure 4.1. Eight node solid hexahedron element. 𝐁 is the 6 × 24 strain-displacement matrix 𝐁 = ∂ ∂𝑥 ⎡ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎣ ∂ ∂𝑦 ∂ ∂𝑧 ∂ ∂𝑦 ∂ ∂𝑥 ∂ ∂𝑧 ∂ ∂𝑧 ⎤ ⎥ ⎥ ⎥ ⎥ ⎥ ⎥ ⎥ ⎥ ⎥ ⎥ ⎥ ⎥ ∂ ⎥ ⎥ ∂𝑦 ⎥ ∂ ⎥ ∂𝑥⎦ 𝐍. (4.5) In order to achieve a diagonal mass matrix the rows are summed giving the kth diagonal term as 𝑚𝑘𝑘 = ∫ 𝜌𝜙𝑘 ∑ 𝜙𝑖𝑑𝜐 = ∫ 𝜌𝜙𝑘𝑑𝜐 , (4.6) 𝑖=1 since the basis functions sum to unity. Terms in the strain-displacement matrix are readily calculated. Note that LS-DYNA Theory Manual Solid Elements ∂𝜙𝑖 ∂𝜉 ∂𝜙𝑖 ∂𝜂 ∂𝜙𝑖 ∂𝜁 = = = ∂𝜙𝑖 ∂𝑥 ∂𝜙𝑖 ∂𝑥 ∂𝜙𝑖 ∂𝑥 ∂𝑥 ∂𝜉 ∂𝑥 ∂𝜂 ∂𝑥 ∂𝜁 + + + ∂𝜙𝑖 ∂𝑦 ∂𝜙𝑖 ∂𝑦 ∂𝜙𝑖 ∂𝑦 ∂𝑦 ∂𝜉 ∂𝑦 ∂𝜂 ∂𝑦 ∂𝜁 + + + ∂𝜙𝑖 ∂𝑧 ∂𝜙𝑖 ∂𝑧 ∂𝜙𝑖 ∂𝑧 ∂𝑧 ∂𝜉 ∂𝑧 ∂𝜂 ∂𝑧 ∂𝜁 , , , which can be rewritten as ∂𝜙𝑖 ⎤ ⎡ ∂𝜉 ⎥ ⎢ ⎥ ⎢ ∂𝜙𝑖 ⎥ ⎢ ⎥ ⎢ ∂𝜂 ⎥ ⎢ ⎥ ⎢ ∂𝜙𝑖 ⎥ ⎢ ∂𝜁 ⎦ ⎣ = ∂𝑥 ∂𝜉 ∂𝑥 ∂𝜂 ∂𝑥 ∂𝜁 ⎡ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎣ ∂𝑦 ∂𝜉 ∂𝑦 ∂𝜂 ∂𝑦 ∂𝜁 ∂𝑧 ⎤ ∂𝜉 ⎥ ⎥ ∂𝑧 ⎥ ⎥ ∂𝜂 ⎥ ⎥ ∂𝑧 ⎥ ∂𝜁 ⎦ ∂𝜙𝑖 ⎤ ⎡ ∂𝑥 ⎥ ⎢ ⎥ ⎢ ∂𝜙𝑖 ⎥ ⎢ ⎥ ⎢ ∂𝑦 ⎥ ⎢ ∂𝜙𝑖 ⎥ ⎢ ∂𝑧 ⎦ ⎣ = 𝐉 ∂𝜙𝑖 ⎤ ⎡ ∂𝑥 ⎥ ⎢ ⎥ ⎢ ∂𝜙𝑖 ⎥ ⎢ . ⎥ ⎢ ∂𝑦 ⎥ ⎢ ∂𝜙𝑖 ⎥ ⎢ ∂𝑧 ⎦ ⎣ Inverting the Jacobian matrix, J, we can solve for the desired terms ∂𝜙𝑖 ⎤ ⎡ ∂𝑥 ⎥ ⎢ ⎥ ⎢ ∂𝜙𝑖 ⎥ ⎢ ⎥ ⎢ ∂𝑦 ⎥ ⎢ ∂𝜙𝑖 ⎥ ⎢ ∂𝑧 ⎦ ⎣ = 𝐉−1 ∂𝜙𝑖 ⎤ ⎡ ∂𝜉 ⎥ ⎢ ⎥ ⎢ ∂𝜙𝑖 ⎥ ⎢ ⎥ ⎢ ∂𝜂 ⎥ ⎢ ⎥ ⎢ ∂𝜙𝑖 ⎥ ⎢ ∂𝜁 ⎦ ⎣ . (4.7) (4.8) (4.9) 4.1 Volume Integration Volume integration is carried out with Gaussian quadrature. If 𝑔 is some function defined over the volume, and 𝑛 is the number of integration points, then ∫ 𝑔𝑑𝜐 = ∫ ∫ ∫ 𝑔|𝐉|𝑑𝜉𝑑𝜂𝑑𝜁 −1 −1 −1 , is approximated by ∑ ∑ ∑ 𝑔𝑗𝑘𝑙∣𝐽𝑗𝑘𝑙∣𝑤𝑗𝑤𝑘𝑤𝑙 𝑗=1 𝑘=1 𝑙=1 , where 𝑤𝑗, 𝑤𝑘, 𝑤𝑙 are the weighting factors, 𝑔𝑗𝑘𝑙 = g(𝜉𝑗, 𝜂𝑘, 𝜁𝑙), and 𝐽 is the determinant of the Jacobian matrix. For one-point quadrature 𝑛 = 1, 𝑤𝑖 = 𝑤𝑗 = 𝑤𝑘 = 2, (4.10) (4.11) (4.12) (4.13) Solid Elements LS-DYNA Theory Manual Strain displacement matrix Strain rates Force Subtotal Hourglass control Total DYNA3D Flanagan Belytschko Wilkins FDM 94 87 117 298 130 428 357 156 195 708 620 1328 843 270 1113 680 1793 Table 4.1. Operation counts for a constant stress hexahedron (includes adds, subtracts, multiplies, and divides in major subroutines, and is independent of vectorization). Material subroutines will add as little as 60 operations for the bilinear elastic-plastic routine to ten times as much for multi-surface plasticity and reactive flow models. Unvectorized material models will increase that share of the cost a factor of four or more. and we can write 𝜉1 = 𝜂1 = 𝜁1 = 0, Note that 8|𝐽(0,0,0)| approximates the element volume. ∫ 𝑔𝑑𝑣 = 8𝑔(0,0,0)|𝐉(0,0,0)|. (4.14) Perhaps the biggest advantage to one-point integration is a substantial savings in computer time. An anti-symmetry property of the strain matrix , , , = − = − = − = − ∂𝜙7 ∂𝑥𝑖 ∂𝜙8 ∂𝑥𝑖 ∂𝜙1 ∂𝑥𝑖 ∂𝜙2 ∂𝑥𝑖 ∂𝜙5 ∂𝑥𝑖 ∂𝜙6 ∂𝑥𝑖 ∂𝜙3 ∂𝑥𝑖 ∂𝜙4 ∂𝑥𝑖 at 𝜉 = 𝜂 = 𝜁 = 0 reduces the amount of effort required to compute this matrix by more than 25 times over an 8-point integration. This cost savings extends to strain and element nodal force calculations where the number of multiplies is reduced by a factor of 16. Because only one constitutive evaluation is needed, the time spent determining stresses is reduced by a factor of 8. Operation counts for the constant stress hexahedron are given in Table 4.1. Included are counts for the Flanagan and Belytschko [1981] hexahedron and the hexahedron used by Wilkins [1974] in his integral finite difference method, which was also implemented [Hallquist 1979]. , (4.15) It may be noted that 8-point integration has another disadvantage in addition to cost. Fully integrated elements used in the solution of plasticity problems and other LS-DYNA Theory Manual Solid Elements problems where Poisson’s ratio approaches 0.5 lock up in the constant volume bending modes. To preclude locking, an average pressure must be used over the elements; consequently, the zero energy modes are resisted by the deviatoric stresses. if the deviatoric stresses are insignificant relative to the pressure or, even worse, if material failure cause loss of this stress state component, hourglassing will still occur, but with no means of resisting it. Sometimes, however, the cost of the fully integrated element may be justified by increased reliability and if used sparingly may actually increase the overall speed. 4.2 Solid Element 2 Solid element 2 is a selective reduced (S/R) integrated element that in general is regarded as too stiff. In particular this is the case when the elements exhibit poor aspect ratio, i.e., when one element dimension is significantly smaller than the other(s). This occurs for instance when modelling thin walled structures and the time for solving the problem prevents using a sufficient number of elements for maintaining close to cubic elements throughout the structure. The reason for the locking phenomenon is that the element is not able to represent pure bending modes without introducing transverse shear strains, and this may be bad enough to lock the element to a great extent. In an attempt to solve this transverse shear locking problem, two new fully integrated solid elements are introduced and documented herein that may become of practical use for these types of applications. 4.2.1 Brief summary of solid element 2 Let 𝑥𝐼𝑖 represent the nodal coordinate of dimension 𝑖 and node 𝐼, and likewise 𝑣𝐼𝑖 its velocity. Furthermore denote 𝑁𝐼(𝜉1, 𝜉2, 𝜉3) = (1 + 𝜉1 𝐼𝜉1 + 𝜉2 𝐼𝜉2 + 𝜉3 𝐼𝜉3 + 𝜉12 𝐼 𝜉1𝜉2 + 𝜉13 𝐼 𝜉1𝜉3 + 𝜉23 𝐼 𝜉2𝜉3 + 𝜉123 𝐼 𝜉1𝜉2𝜉3),(4.2.16) the shape functions for the standard isoparametric domain where 1 −1 −1 ∗ = [−1 𝜉1 ∗ = [−1 −1 𝜉2 1 −1 −1 ∗ = [−1 −1 −1 −1 𝜉3 ∗ = [ 1 −1 𝜉12 1 −1 1 −1 ∗ = [ 1 −1 −1 𝜉13 1 −1 ∗ = [ 1 𝜉23 1 −1 −1 −1 −1 ∗ = [−1 𝜉123 1 −1 1 −1 and let furthermore 1 −1], 1], 1], 1 −1], 1 −1], 1], 1 −1], 𝐼 , 𝐼 = 𝜉12 𝜉21 𝐼 = 𝜉23 𝐼 , 𝜉32 𝐼 . 𝐼 = 𝜉13 𝜉31 (4.2.17) (4.2.18) Solid Elements LS-DYNA Theory Manual Figure 4.2.2. Bending mode for a fully integrated brick. The isoparametric representation of the coordinates of a material point in the element is then given as (where the dependence on 𝜉1, 𝜉2, 𝜉3 is suppressed for brevity) and its associated jacobian matrix is 𝑥𝑖 = 𝑥𝐼𝑖𝑁𝐼, 𝐽𝑖𝑗 = 𝜕𝑥𝑖 𝜕𝜉𝑗 = 𝑥𝐼𝑖 (𝜉𝑗 𝐼 + 𝜉𝑗𝑘 𝐼 𝜉𝑘 + 𝜉𝑗𝑙 𝐼 𝜉𝑙 + 𝜉123 𝐼 𝜉𝑘𝜉𝑙), (4.2.19) (4.2.20) where 𝑘 = 1 + mod(𝑗, 3) and 𝑙 = 1 + mod(𝑗 + 1,3). For future reference let be the jacobian evaluated in the element center and in the beginning of the simulation (i.e., at time zero). The velocity gradient computed directly from the shape functions and velocity components is 0 = 𝑥𝐼𝑖(0) 𝐽𝑖𝑗 (4.2.21) 𝐼, 𝜉𝑗 where 𝐿𝑖𝑗 = 𝜕𝑣𝑖 𝜕𝑥𝑗 = 𝐽 ̇𝑖𝑘𝐽𝑘𝑗 −1 = 𝐵𝑖𝑗𝐼𝑘𝑣𝐼𝑘, 𝐵𝑖𝑗𝐼𝑘 = 𝜕𝑁𝐼 𝜕𝜉𝑙 −1𝛿𝑖𝑘, 𝐽𝑙𝑗 (4.2.22) (4.2.23) is the gradient-displacement matrix and represents the element except for the alleviation of volumetric locking. To do just that, let 𝐵𝑖𝑗𝐼𝑘 0 be defined by 0 𝑣𝐼𝑘, with 𝐽 ̅𝑖𝑗 being the element averaged jacobian matrix, and construct the gradient- displacement matrix used for the element as −1 = 𝐵𝑖𝑗𝐼𝑘 𝑖𝑘𝐽 ̅ 𝐽 ̅ 𝑘𝑗 (4.2.24) 𝐵̅̅̅̅𝑖𝑗𝐼𝑘 = 𝐵𝑖𝑗𝐼𝑘 + (𝐵𝑙𝑙𝐼𝑘 0 − 𝐵𝑙𝑙𝐼𝑘)𝛿𝑖𝑗. (4.2.25) This is what is often called the B-bar method. 4-6 (Solid Elements) LS-DYNA Theory Manual Solid Elements 4.2.2 Transverse shear locking example To get the idea of the modifications needed to alleviate transverse shear locking let’s look at the parallelepiped of dimensions 𝑙1 × 𝑙2 × 𝑙3 in the Figure above. For this simple geometry the jacobian matrix is diagonal and the velocity gradient is expressed as 𝐿𝑖𝑗 = 𝑙𝑗 𝐽 ̇𝑖𝑗 = 4𝑙𝑗 𝑣𝐼𝑖(𝜉𝑗 𝐼 + 𝜉𝑗𝑘 𝐼 𝜉𝑘 + 𝜉𝑗𝑙 𝐼 𝜉𝑙 + 𝜉123 𝐼 𝜉𝑘𝜉𝑙), (4.2.26) where, again, 𝑘 = 1 + mod(𝑗, 3) and 𝑙 = 1 + mod(𝑗 + 1,3). Now let 𝑖 ≠ 𝑝 ≠ 𝑞 ≠ 𝑖, then a pure bending mode in the plane with normal in direction 𝑞 and about axis 𝑝 is represented by 𝐼 , 𝑣𝐼𝑖 = 𝜉𝑖𝑞 𝑣𝐼𝑝 = 0, 𝑣𝐼𝑞 = 0, and thus the velocity gradient is given as (𝜉𝑖𝑞 𝐼 𝜉𝑗𝑘 𝐼 𝜉𝑘 + 𝜉𝑖𝑞 𝐼 𝜉𝑗𝑙 𝐼 𝜉𝑙), 𝐿𝑖𝑗 = 4𝑙𝑗 𝐿𝑝𝑗 = 0, 𝐿𝑞𝑗 = 0, for 𝑗 = 1, 2, 3. The nonzero expression above amounts to 𝐿𝑖𝑖 = 4𝑙𝑖 𝐿𝑖𝑝 = 0, 4𝑙𝑞 𝐿𝑖𝑞 = 𝜉𝑞, 𝜉𝑖. (4.2.27) (4.2.28) (4.2.29) Notable here is that a pure bending mode gives arise to a transverse shear strain represented by the last expression in the above. Assuming that 𝑙𝑞 is small compared to 𝑙𝑖 this may actually lock the element. 4.2.3 Solid element -2 Given this insight the modifications in the expression of the jacobian matrix are as follows. Let 𝜅𝑚𝑛 = min 0 + 𝐽2𝑚 0 + 𝐽2𝑛 be the aspect ratio between dimensions 𝑚 and 𝑛 at time zero. The modified jacobian is written 0 + 𝐽3𝑚 0 + 𝐽3𝑛 0 𝐽3𝑚 0 𝐽3𝑛 0 𝐽1𝑚 0 𝐽1𝑛 0 𝐽2𝑚 0 𝐽2𝑛 √𝐽1𝑚 √𝐽1𝑛 ⎜⎜⎜⎛ ⎝ ⎟⎟⎟⎞ ⎠ (4.2.30) 1, , 𝐽 ̃𝑖𝑗 = 𝑥𝐼𝑖 where LS-DYNA Draft (𝜉𝑗 𝐼 + 𝜉𝑗𝑘 𝐼 𝜉𝑘𝑖 + 𝜉𝑗𝑙 𝐼 𝜉𝑙𝑖 + 𝜉123 𝐼 𝜉𝑘𝑖𝜉𝑙𝑖), Solid Elements LS-DYNA Theory Manual and 𝜉𝑘𝑖 = { 𝜉𝑘𝜅𝑗𝑘 𝜉𝑘 𝑖 ≠ 𝑗 otherwise , 𝜉𝑙𝑖 = { 𝜉𝑙𝜅𝑗𝑙 𝜉𝑙 𝑖 ≠ 𝑗 otherwise . The velocity gradient is now given as (4.2.32) (4.2.33) −1 = 𝐵̃ 𝑖𝑗𝐼𝑘𝑣𝐼𝑘, 𝑖𝑘𝐽 ̃ 𝑘𝑗 where 𝐵̃ 𝑖𝑗𝐼𝑘 is the gradient-displacement matrix used for solid element type -2 in LS- DYNA. The B-bar method is used to prevent volumetric locking. 𝐿𝑖𝑗 = 𝐽 ̃ (4.2.34) 4.2.4 Transverse shear locking example revisited Once again let’s look at the parallelepiped of dimensions 𝑙1 × 𝑙2 × 𝑙3. The jacobian matrix is still diagonal and the velocity gradient is with the new element formulation expressed as 𝐿𝑖𝑗 = 𝑙𝑗 𝐽 ̃ 𝑖𝑗 = 4𝑙𝑗 𝑣𝐼𝑖(𝜉𝑗 𝐼 + 𝜉𝑗𝑘 𝐼 𝜉𝑘𝑖 + 𝜉𝑗𝑙 𝐼 𝜉𝑙𝑖 + 𝜉123 𝐼 𝜉𝑘𝑖𝜉𝑙𝑖), (4.2.35) where, again, 𝑘 = 1 + mod(𝑗, 3) and 𝑙 = 1 + mod(𝑗 + 1,3). The velocity gradient for a pure bending mode is now given as 𝐿𝑖𝑗 = 4𝑙𝑗 (𝜉𝑖𝑞 𝐼 𝜉𝑗𝑘 𝐼 𝜉𝑘𝑖 + 𝜉𝑖𝑞 𝐼 𝜉𝑗𝑙 𝐼 𝜉𝑙𝑖), which amounts to (for the potential nonzero elements) 𝜉𝑞, 𝐿𝑖𝑖 = 4𝑙𝑖 𝐿𝑖𝑝 = 0, 4𝑙𝑞 𝐿𝑖𝑞 = 𝜉𝑖𝜅𝑞𝑖. (4.2.36) (4.2.37) If we assume that this is the geometry in the beginning of the simulation and that 𝑙𝑞 is smaller than 𝑙𝑖 the transverse shear strain can be expressed as meaning that the transverse shear energy is not affected by poor aspect ratios, i.e., the transverse shear strain does not grow with decreasing 𝑙𝑞. 𝐿𝑖𝑞 = 4𝑙𝑖 𝜉𝑖, (4.2.38) 4.2.5 Solid element -1 Working out the details in the expression of the gradient-displacement matrix for solid element type -2 reveals that this matrix is dense, i.e., there are 216 nonzero elements in 4-8 (Solid Elements) LS-DYNA Draft LS-DYNA Theory Manual Solid Elements this matrix that needs to be processed compared to 72 for the standard solid element type 2. A slight modification of the jacobian matrix will substantially reduce the computational expense for this element. Simply substitute the expressions for 𝜉𝑘𝑖 and 𝜉𝑙𝑖 by and 𝜉𝑘𝑖 = 𝜉𝑘𝜅𝑗𝑘, 𝜉𝑙𝑖 = 𝜉𝑙𝜅𝑗𝑙. (4.2.39) (4.2.40) This will lead to a stiffness reduction for certain modes, in particular the out-of- plane hourglass mode as can be seen by once again looking at the transverse shear locking example. The velocity gradient for pure bending is now 𝐿𝑖𝑖 = 4𝑙𝑖 𝐿𝑖𝑝 = 0, 4𝑙𝑞 𝐿𝑖𝑞 = 𝜉𝑞𝜅𝑖𝑞, 𝜉𝑖𝜅𝑞𝑖, and if it turns out that 𝑙𝑖 is smaller than 𝑙𝑞, then this results in 𝐿𝑖𝑖 = 4𝑙𝑞 𝜉𝑞. (4.2.41) (4.2.42) That is, if 𝑖 represents the direction of the thinnest dimension, its corresponding bending strain is inadequately reduced. 4.2.6 Example A plate of dimensions 10 × 5 × 1 mm3 is clamped at one end and subjected to a 1 Nm torque at the other end. The Young’s modulus is 210 GPa and the analytical solution for the end tip deflection is 0.57143 mm. In order to study the mesh convergence for the three fully integrated bricks the plate is discretized into 2 × 1 × 1, 4 × 2 × 2, 8 × 4 × 4, 16 × 8 × 8and finally 32 × 16 × 16 elements, all elements having the same aspect ratio of 5 × 1. The table below shows the results for the different fully integrated elements, and indicates an accuracy improvement for solid elements −1 and −2. Discretization Solid element type 2 2x1x1 4x2x2 8x4x4 16x8x8 32x16x16 Solid element type -2 Solid element type -1 0.6711 (17.4%) 0.5466 (4.3%) 0.5472 (4.2%) 0.5516 (3.5%) 0.5535 (3.1%) 0.0564 (90.1%) 0.1699 (70.3%) 0.3469 (39.3%) 0.4820 (15.7%) 0.5340 (6.6%) 0.6751 (18.1%) 0.5522 (3.4%) 0.5500 (3.8%) 0.5527 (3.3%) 0.5540 (3.1%) 4.3 Hourglass Control The biggest disadvantage to one-point integration is the need to control the zero energy modes, which arise, called hourglassing modes. Undesirable hourglass modes tend to have periods that are typically much shorter than the periods of the structural Solid Elements LS-DYNA Theory Manual response, and they are often observed to be oscillatory. However, hourglass modes that have periods that are comparable to the structural response periods may be a stable kinematic component of the global deformation modes and must be admissible. One way of resisting undesirable hourglassing is with a viscous damping or small elastic stiffness capable of stopping the formation of the anomalous modes but having a negligible affect on the stable global modes. Two of the early three-dimensional algorithms for controlling the hourglass modes were developed by Kosloff and Frazier [1974] and Wilkins et al. [1974]. Since the hourglass deformation modes are orthogonal to the strain calculations, work done by the hourglass resistance is neglected in the energy equation. This may lead to a slight loss of energy; however, hourglass control is always recommended for the under integrated solid elements. The energy dissipated by the hourglass forces reacting against the formations of the hourglass modes is tracked and reported in the output files matsum and glstat. It is easy to understand the reasons for the formation of the hourglass modes. Consider the following strain rate calculations for the 8-node solid element 𝜀̇𝑖𝑗 = (∑ 𝑘=1 ∂𝜙𝑘 ∂𝑥𝑖 𝑥̇𝑗 + ∂𝜙𝑘 ∂𝑥𝑗 𝑘). 𝑥̇𝑖 Whenever diagonally opposite nodes have identical velocities, i.e., 7, 1 = 𝑥̇𝑖 𝑥̇𝑖 8, 2 = 𝑥̇𝑖 𝑥̇𝑖 5, 3 = 𝑥̇𝑖 𝑥̇𝑖 6, 4 = 𝑥̇𝑖 𝑥̇𝑖 (4.43) (4.44) 1k 3k 2k 4k Figure 4.3. The hourglass modes of an eight-node element with one integration point are shown [Flanagan and Belytschko 1981]. A total of twelve modes exist. LS-DYNA Theory Manual Solid Elements 𝛼 = 1 𝛼 = 2 𝛼 = 3 𝛼 = 4 1 -1 1 -1 -1 1 -1 1 1 -1 -1 1 -1 1 1 -1 1 -1 1 -1 1 -1 1 -1 1 1 -1 -1 -1 -1 1 1 𝛤𝑗1 𝛤𝑗2 𝛤𝑗3 𝛤𝑗4 𝛤𝑗5 𝛤𝑗6 𝛤𝑗7 𝛤𝑗8 Table 4. Hourglass base vectors. the strain rates are identically zero: 𝜀̇𝑖𝑗 = 0, (4.45) due to the asymmetries in Equations (4.15). It is easy to prove the orthogonality of the hourglass shape vectors, which are listed in Table 4 and shown in Figure 4.3 with the derivatives of the shape functions: ∑ 𝑘=1 ∂𝜙𝑘 ∂𝑥𝑖 𝛤𝛼𝑘 = 0 , 𝑖 = 1, 2, 3, 𝛼 = 1, 2, 3, 4. (4.46) The product of the base vectors with the nodal velocities is zero when the element velocity field has no hourglass component, ℎ𝑖𝛼 = ∑ 𝑥̇𝑖 𝑘𝛤𝛼𝑘 = 0. (4.47) 𝑘 are nonzero if hourglass modes are present. The 12 hourglass-resisting force vectors, 𝑓𝑖𝛼 are 𝑘=1 where 𝑘 = 𝑎ℎℎ𝑖𝛼𝛤𝛼𝑘, 𝑓𝑖𝛼 3⁄ 𝑐 𝑎ℎ = 𝑄HG𝜌𝑣e , (4.48) (4.49) in which 𝑣e is the element volume, 𝑐 is the material sound speed, and 𝑄HG is a user- defined constant usually set to a value between .05 and .15. Equation (1.21) is hourglass control type 1 in the LS-DYNA User’s Manual. A shortcoming of hourglass control type 1 is that the hourglass resisting forces of Equation (1.21) are not orthogonal to linear velocity field when elements are not in the shape of parallelpipeds. As a consequence, such elements can generate hourglass energy with a constant strain field or rigid body rotation. Flanagan and Belytschko [1981] developed an hourglass control that is orthogonal to all modes except the zero energy hourglass modes. Instead of resisting components of the bilinear velocity field that are orthogonal to the strain calculation, Flanagan and Belytschko resist components Solid Elements LS-DYNA Theory Manual of the velocity field that are not part of a fully linear field. They call this field, defined below, the hourglass velocity field 𝑘HG 𝑥̇𝑖 = 𝑥̇𝑖 𝑘 − 𝑥̇𝑖 𝑘LIN , where and 𝑘LIN 𝑥̇𝑖 = 𝑥̅ ̇i + 𝑥̅ ̇𝑖,𝑗(𝑥𝑗 𝑘 − 𝑥̅𝑗), 𝑥̅𝑖 = ̇𝑖 = 𝑥̅ 𝑘, ∑ 𝑥𝑖 𝑘=1 ∑ 𝑥̇𝑖 𝑘=1 . (4.50) (4.51) (4.52) Flanagan and Belytschko construct geometry-dependent hourglass shape vectors that are orthogonal to the fully linear velocity field and the rigid body field. With these vectors they resist the hourglass velocity deformations. Defining hourglass shape vectors in terms of the base vectors as the analogue for (4.47) is, 𝛾𝛼𝑘 = 𝛤𝛼𝑘 − 𝜙𝑘,𝑖 ∑ 𝑥𝑖 𝛤𝛼𝑛, 𝑛=1 𝑔𝑖𝛼 = ∑ 𝑥̇𝑖 𝑘=1 𝛾𝛼𝑘 = 0, with the 12 resisting force vectors being 𝑘 = 𝑎ℎ𝑔𝑖𝛼𝛾𝛼𝑘, 𝑓𝑖𝛼 (4.53) (4.54) (4.55) where 𝑎ℎ is a constant given in Equation (4.48). Equation (1.28) corresponds to hourglass control type 2 in the LS-DYNA User’s Manual. The 𝛾 terms used of equation of Equation (1.26) are used not only type hourglass control type 2, but are the basis for all solid element hourglass control except for form 1. A cost comparison in Table 4.1 shows that the default type 1 hourglass viscosity requires approximately 130 adds or multiplies per hexahedron, compared to 620 and 680 for the algorithms of Flanagan-Belytschko and Wilkins. Therefore, for a very regular mesh, type 1 hourglass control may provide a faster, sufficiently accurate solution, but in general, any of the other hourglass options which are all based on the 𝛾𝛼𝑘 terms of Equation (1.26) will be a better choice. Type 3 hourglass control is identical to type 2, except that the shape function derivatives in Eq. (1.26) are evaluated at the centroid of the element rather than at the origin of the referential coordinate system. With this method, Equation (1.14) produces the exact element volume. However, the anti-symmetry property of Equation (1.15) is not true, so there is some increased number of computations. LS-DYNA Theory Manual Solid Elements The remaining hourglass control types calculated hourglass forces proportional to total hourglass deformation rather than hourglass viscosity. A stiffness form of hourglass control allows elements to spring back and will absorb less energy than the viscous forms. Types 4 and 5 hourglass control are similar to types 2 and 3, except that they evaluate hourglass stiffness rather than viscosity. The hourglass rates of equation (1.27) are multiplied by the solution time step to produce increments of hourglass deformation. The hourglass stiffness is scaled by the element’s maximum frequency so that stability can is maintained as long as the hourglass scale factor, 𝑎ℎ, is sufficiently small. Type 6 hourglass control improves on type 5 by scaling the stiffness such that the hourglass forces match those generated by a fully integrated element control by doing closed form integration over the element volume scaling the hourglass stiffness by matching the stabilization for the 3D hexahedral element is available for both implicit and explicit solutions. Based on material properties and element geometry, this stiffness type stabilization is developed by an assumed strain method [Belytschko and Bindeman 1993] such that the element does not lock with nearly incompressible material. When the user defined hourglass constant 𝑎h is set to 1.0, accurate coarse mesh bending stiffness is obtained for elastic material. For nonlinear material, a smaller value of 𝑎h is suggested and the default value is set to 0.1. In the implicit form, the assumed strain stabilization matrix is: 𝐊stab = 2𝜇𝑎h 𝐤11 𝐤12 𝐤13 ⎤ 𝐤21 𝐤22 𝐤23 , ⎥ 𝐤31 𝐤32 𝐤33⎦ ⎡ ⎢ ⎣ where the 8 × 8 submatricies are calculated by: 𝐤𝑖𝑖 ≡ 𝐻𝑖𝑖 [( ) (𝛄𝑗𝛄𝑗 𝐤𝑖𝑗 ≡ 𝐻𝑖𝑗 [( , ) 𝛄𝑗𝛄𝑖 T + 1 − 𝜐 1 − 𝜐 T + 𝛄𝑘𝛄𝑘 𝛄𝑖𝛄𝑗 T] T) + ( 1 + 𝜐 ) 𝛄4𝛄4 T] + (𝐻𝑗𝑗 + 𝐻𝑘𝑘)𝛄𝑖𝛄1 T, with, where, 𝐻𝑖𝑖 ≡ ∫(ℎ𝑗,𝑖) 𝐻𝑖𝑗 ≡ ∫ ℎ𝑖,𝑗ℎ𝑗,𝑖 𝑑𝑣 = ∫(ℎ𝑘,𝑖)2 𝑑𝑣 = 3 ∫(ℎ4,𝑖)2 𝑑𝑣, 𝑑𝑣, ℎ1 = 𝜉𝜂 ℎ2 = 𝜂𝜁 ℎ3 = 𝜁𝜉 ℎ4 = 𝜉𝜂𝜁 , (4.56) (4.57) (4.58) (4.59) Subscripts 𝑖, 𝑗, and 𝑘 are permuted as in Table 44.2. A comma indicates a derivative with respect to the spatial variable that follows. The hourglass vectors, 𝛾𝛼 are defined by equation (4.53). The stiffness matrix is evaluated in a corotational Solid Elements LS-DYNA Theory Manual 1 1 2 2 3 3 2 3 3 1 1 2 3 2 1 3 2 1 Table 44.2. Permutations of i, j, and k. coordinate system that is aligned with the referential axis of the element. The use of a corotational system allows direct evaluation of integrals in equations (4.58) by simplified equations that produce a more accurate element than full integration. T𝐱𝑗)(𝚲𝑘 T𝐱𝑖) (𝚲𝑖 𝑖 ≠ 𝑗 ≠ 𝑘, 𝐻𝑖𝑖 = T𝐱𝑘) (𝚲𝑗 (4.60) 𝐻𝑖𝑗 = (𝚲𝑘 T𝐱𝑘) 𝑖 ≠ 𝑗 ≠ 𝑘, (4.61) Λ𝑖 are 8 × 1 matrices of the referential coordinates of the nodes as given in Figure 4.1, and x𝑖 are 8 × 1 matrices of the nodal coordinates in the corotational system. For each material type, a Poisson's ratio, 𝑣, and an effective shear modulus, 𝜇, is needed. In the explicit form, the 12 hourglass force stabilization vectors are stab = ∑ 𝑎h𝑔𝑖𝛼𝛄𝛼 𝐟𝑖 𝛼=1 , where the 12 generalized stresses are calculated incrementally by 𝑛 = 𝑔𝑖𝛼 𝑔𝑖𝛼 𝑛−1 + Δ𝑡𝑔̇𝑖𝛼 𝑛−1 2, 𝑔̇𝑖𝑖 = 𝜇[(𝐻𝑗𝑗 + 𝐻𝑘𝑘)𝑞 ̇𝑖𝑖 + 𝐻𝑖𝑗𝑞 ̇𝑗𝑗 + 𝐻𝑖𝑘𝑞 ̇𝑘𝑘], , 𝑔̇𝑖𝑗 = 2𝜇 [ , 𝑔̇𝑖4 = 2𝜇 ( 1 − 𝜐 1 + 𝜈 𝐻𝑖𝑖𝑞 ̇𝑖𝑗 + 𝜐𝐻𝑘𝑘𝑞 ̇𝑖𝑖] ) 𝐻𝑖𝑖𝑞 ̇𝑖4 and where, (4.62) (4.63) (4.64) T𝐱̇𝑖). Subscripts 𝑖, 𝑗, and 𝑘 are permuted as per Table 44.2. As with the implicit form, calculations are done in a corotational coordinate system in order to use the simplified equations (4.60) and (4.61). 𝑞 ̇𝑖𝛼 = (𝛄𝛼 (4.65) LS-DYNA Theory Manual Solid Elements Type 7 hourglass control is very similar to type 6 hourglass control but with one significant difference. As seen in Equation (1.36), type 6 obtains the current value of the generalized stress from the previous value and the current increment. The incremental method is nearly always sufficiently accurate, but it is possible for hourglass modes to fail to spring back to the initial element geometry since the hourglass stiffness varies as the H terms given by Equations (1.33) and (1.34) are recalculated in the deformed configuration each cycle. Type 7 hourglass control eliminates this possible error by calculating the total hourglass deformation in each cycle. For type 7 hourglass control, Equations (1.37) are rewritten using 𝑔 and 𝑞 in place of 𝑔̇ and 𝑞 ̇, and Equation (1.38) is replaced by (1.39). 𝑞𝑖𝛼 = (𝛄𝛼 T𝐱𝑖) − (𝛄0𝛼 In Equation (1.39), 𝐱𝟎𝒊 and 𝛄𝟎𝜶 are evaluated using the initial, undeformed nodal coordinate values. Type 7 hourglass control is considerably slower than type 6, so it is not generally recommended, but may be useful when the solution involves at least several cycles of loading and unloading that involve large element deformation of elastic or hyperelastic material. T 𝐱0𝑖). (4.39) Both type 6 and 7 hourglass control are stiffness type methods, but may have viscosity added through the VDC parameter on the *HOURGLASS card. The VDC parameter scales the added viscosity, and VDC = 1.0 corresponds approximately to critical damping. The primary motivation for damping is to reduce high frequency oscillations. A small percentage of critical damping should be sufficient for this, but it is also possible to add supercritical damping along with a small value of QM to simulate a very viscous material that springs back slowly. 4.4 Puso Hourglass Control Regarding the solid elements in LS-DYNA, the fully integrated brick uses selective-reduced integration, which is known to alleviate volumetric locking but not shear locking for elements with poor aspect ratio. The enhanced assumed strain methods have been the most successful at providing coarse mesh accuracy for general non-linear material models. In short, these elements tend to sacrifice computational efficiency for accuracy and are hence of little interest in explicit analysis. Puso [2000] developed an enhanced assumed strain element that combines coarse mesh accuracy with computational efficiency. It is formulated as a single point integrated brick with In this project, we have an enhanced assumed strain physical stabilization. implemented this element in LS-DYNA and made comparisons with the assumed strain element developed by Belytschko and Bindeman [1993] to see whether it brings anything new to the existing LS-DYNA element library. This is hourglass control type 9. Solid Elements LS-DYNA Theory Manual The element formulation is that of Puso [2000], and is essentially the mean strain hexahedral element by Flanagan and Belytschko [1981] in which the perturbation hourglass control is substituted for an enhanced assumed strain stabilization force. Given the matrices 𝐒 = ⎤ ⎡ ⎥ ⎢ ⎥ ⎢ ⎥ ⎢ ⎥ ⎢ ⎥ ⎢ ⎥ ⎢ ⎥ ⎢ ⎥ ⎢ 1⎦ ⎣ , 𝚵 = −1 −1 −1 ⎤ 1 −1 −1 ⎥ 1 −1 ⎥ ⎥ 1 −1 −1 ⎥ ⎥ −1 −1 ⎥ 1 −1 ⎥ ⎥ 1⎦ −1 ⎡ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎣ , 𝐇 = we can define the vector of shape functions as 1 −1 −1 1 −1 ⎤ ⎥ −1 −1 1 −1 ⎥ ⎥ −1 1 −1 ⎥ , ⎥ −1 −1 ⎥ −1 1 −1 −1 ⎥ ⎥ 1 −1 −1 −1⎦ ⎡ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎣ where The position vector 𝐍(𝛏) = [𝐬 + 𝚵𝛏 + 𝐇𝐡(𝛏)], 𝛏 = ⎤ , ⎡ ⎥ ⎢ 𝜍⎦ ⎣ 𝐡(𝛏) = 𝜂𝜍 ⎤ 𝜉𝜍 ⎥⎥⎥ . 𝜉𝜂 𝜉𝜂𝜍⎦ ⎡ ⎢⎢⎢ ⎣ 𝐱(𝛏) = 𝑥(𝛏) ⎤ 𝑦(𝛏) , ⎥ 𝑧(𝛏)⎦ ⎡ ⎢ ⎣ is for isoparametric finite elements given as 𝐱(𝛏) = 𝐗T𝐍(𝛏), where (4.66) (4.67) (4.68) (4.69) (4.70) 𝑦1 𝑦2 𝑦3 𝑦4 𝑦5 𝑦6 𝑦7 𝑦8 is the matrix of nodal coordinates. The Jacobian matrix maps the isoparametric domain to the physical domain as 𝑧1 ⎤ 𝑧2 ⎥ 𝑧3 ⎥ ⎥ 𝑧4 ⎥ , 𝑧5 ⎥ ⎥ 𝑧6 ⎥ ⎥ 𝑧7 𝑧8⎦ 𝑥1 ⎡ 𝑥2 ⎢ 𝑥3 ⎢ ⎢ 𝑥4 ⎢ 𝑥5 ⎢ ⎢ 𝑥6 ⎢ ⎢ 𝑥7 𝑥8 ⎣ 𝐗 = (4.71) and we find the Jabobian matrix at the element centroid to be 𝐉(𝛏) = ∂𝐱(𝛏) ∂𝛏 , (4.72) LS-DYNA Theory Manual Solid Elements We may use this to rewrite the vector of shape functions partially in terms of the position vector as 𝐉0 = 𝐉(0) = 𝐗T𝚵. (4.73) Where 𝐍(𝛏) = 𝐛0 + 𝐁0𝐱 + 𝚪𝐡(𝛏), 𝐛0 = 𝚪 = 𝐁0 = {𝐈 − 𝐁0𝐗T}𝐬 , {𝐈 − 𝐁0𝐗T}𝐇, −1 𝚵𝐉0 . The gradient-displacement matrix from this expression is given as where We have 𝐁(𝛏) = 𝐁0 + 𝐁𝑠(𝛏), 𝐁𝑠(𝛏) = 𝚪 ∂𝐡(𝛏) ∂𝛏 𝐉(𝛏)−1. ∂𝐡(𝛏) ∂𝛏 = 𝜂𝜍 ⎡ ⎢ ⎢ ⎢ ⎣ 𝜉𝜍 ⎤ ⎥ . ⎥ ⎥ 𝜉𝜂⎦ (4.74) (4.75a) (4.75b) (4.75c) (4.76) (4.77) (4.78) At this point we substitute the gradient-displacement matrix at the centroid of the element 𝐁0 with the mean gradient-displacement matrix 𝐁 defined as 𝐁 = 𝑉𝑒 ∫ 𝐁(𝛏)𝑑𝑉𝑒 , (4.79) where 𝑒 refers to the element domain and 𝑉𝑒 is the volume of the element, in all of the expressions above. That is and where 𝚪 = {𝐈 − 𝐁𝐗T}𝐇, 𝐁(𝛏) = 𝐁 + 𝐁𝑠(𝛏), 𝐁𝑠(𝛏) = 𝚪 ∂𝐡(𝛏) ∂𝛏 𝐉(𝛏). Proceeding, we write the expression for the rate-of-deformation as (4.80) (4.81) (4.82) Solid Elements LS-DYNA Theory Manual 𝛆̇ = = = = [𝐗̇ T𝐁(𝛏) + 𝐁(𝛏)T𝐗̇] (𝐗̇ T 𝐁 + 𝐁 (𝐗̇ T 𝐁 + 𝐁 𝐗̇ ) + 𝐗̇ ) + (𝐗̇ T 𝐁 + 𝐁 𝐗̇) + 𝐗̇ T𝚪 [𝐗̇ T𝐁𝑠(𝛏) + 𝐁𝑠(𝛏)T𝐗̇ ] {⎧ 2 ⎩{⎨ 𝐉(𝛏)−T ∂𝐡(𝛏) ∂𝛏 {⎧ ⎩{⎨ 𝐉(𝛏)T𝐗̇ T𝚪 ∂𝐡(𝛏) ∂𝛏 𝐉(𝛏)−1 + 𝐉(𝛏)−T [ ∂𝐡(𝛏) ∂𝛏 ∂𝐡(𝛏) ∂𝛏 ] ] 𝐗̇ }⎫ ⎭}⎬ }⎫ 𝐗̇𝐉(𝛏) ⎭}⎬ + [ (4.83) 𝐉(𝛏)−1, where we substitute the occurrences of the jacobian matrix 𝐉(ξ)with the following expressions 𝛆̇ ≈ (𝐗̇ T 𝐁 + 𝐁 𝐗̇) + −T 𝐉̂0 {⎧ ⎩{⎨ T𝐗̇ T𝚪 𝐉0 ∂𝐡(𝛏) ∂𝛏 + [ ∂𝐡(𝛏) ] ∂𝛏 𝚪T𝐗̇𝐉0 }⎫ ⎭}⎬ −1, 𝐉̂0 where 𝐉̂0 = ∥𝐣1∥ ⎡ ⎢ ⎣ ∥𝐣2∥ ⎤ , ⎥ ∥𝐣3∥⎦ (4.84) (4.85) and j𝑖 is the i:th column in the matrix 𝐉0. This last approximation is the key to the mesh distortion insensitivity that characterizes the element. Changing to Voigt notation, we define the stabilization portion of the strain rate as where now −1 = 𝐉0 ∥𝐣1∥−2 ⎡ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎣ 𝛆̇𝑠 = 𝐉̂0 −1𝐁̃𝑠(𝛏)𝐮̇ ̃, ∥𝐣2∥−2 ∥𝐣3∥−2 ∥𝐣1∥−1∥𝐣2∥−1 ∥𝐣3∥−1∥𝐣2∥−1 ⎤ ⎥ ⎥ ⎥ ⎥ , ⎥ ⎥ ⎥ ⎥ ⎥ ∥𝐣1∥−1∥𝐣3∥−1⎦ 𝐁̃𝑠(𝛏) = γ2𝜍 + γ3𝜂 + γ4𝜍𝜂 ⎡ ⎢ ⎢ ⎢ ⎢ γ1𝜍 ⎢ ⎢ ⎢ γ1𝜂 ⎣ γ1𝜍 + γ3𝜉 + γ4𝜍𝜉 γ2𝜍 γ2𝜉 γ1𝜂 + γ2𝜉 + γ4𝜉𝜂 γ3𝜉 γ3𝜂 ⎤ ⎥ ⎥ ⎥ , ⎥ ⎥ ⎥ ⎥ ⎦ (4.86) (4.87) (4.88) ̃ is the vector of nodal velocities transformed to the isoparametric system and 𝐮̇ according to LS-DYNA Theory Manual Solid Elements where 𝕵 is the 24 × 24 matrix that transforms the 8 nodal velocity vectors to the isoparametric domain given by 𝐮̇ ̃ = 𝕵𝐮̇, (4.89) 𝕵 = perm 𝐉0 ⎡ ⎢⎢ ⎣ ⋱ ⎤ . ⎥⎥ T⎦ 𝐉0 (4.90) Moreover, 𝛄𝑖 is the ith row of 𝚪 parallelepiped finite elements to lock in shear. . We have deliberately neglected terms that cause To eliminate Poisson type locking in bending and volumetric locking, an enhanced isoparametric rate-of-strain field is introduced as with 𝛆̇𝑒 = 𝐉̂0 −1𝐆̃(𝛏)𝛂̇, 𝜂 0 Hence, the stabilized strain field becomes 𝐆̃(𝛏) = ⎡ ⎢ ⎢ ⎢ ⎢ ⎢ ⎣ 𝜉𝜂 𝜂𝜍 𝜉𝜂 𝜂𝜍 𝜉𝜂 𝜂𝜍 𝜍𝜉 ⎤ 𝜍𝜉 ⎥ ⎥ 𝜍𝜉 . ⎥ ⎥ ⎥ 0 ⎦ 𝛆̇𝑠 = 𝐉̂0 −1[𝐁̃𝑠(𝛏)𝐮̇ ̃ + 𝐆̃(𝛏)𝛂̇] = 𝐉̂0 −1𝛆̇ ̃𝑠, (4.91) (4.92) (4.93) where 𝜶̇ is the enhanced strain vector that must be determined from an equilibrium condition. The virtual work equation can be written 𝛿𝑊int = ∫ 𝛿𝛆T𝛔𝐝𝑉𝑒 , = ∫ 𝛿𝛆T𝐽−1𝐉T𝐒𝑑𝑉𝑒 , = ∫ 𝛿𝛆T𝐽−1𝐉T = ∫ 𝛿𝛆T𝐽−1𝐉T ⎜⎛∫ 𝐂𝑆𝐸𝐄̇𝑑𝜏 ⎝ ⎟⎞ 𝑑𝑉𝑒 ⎠ , ⎜⎛∫ 𝐽𝐉−T𝐂𝜎𝛆̇𝑑𝜏 ⎝ ⎟⎞ 𝑑𝑉𝑒 ⎠ , = ∫ 𝛿𝛆T𝑗0𝐉0 ≈ ∫ 𝛿𝛆̃T ⎜⎛∫ ⎝ ⎜⎛∫ 𝐽𝐉0 ⎝ 𝑉𝑒 −T𝐂𝜎𝛆̇𝑑𝜏 ⎟⎞ 𝑑𝑉𝑝 ⎠ , −T𝐂𝜎𝐉̂0 𝐉̂0 −1𝛆̇ ̃𝑑𝜏 ⎟⎞ 𝑑𝑉𝑝 ⎠ , (4.94a) (4.94b) (4.94c) (4.94d) (4.94e) (4.94f) Solid Elements LS-DYNA Theory Manual where 𝐽 is the determinant of the deformation gradient, 𝐉 is the push-forward operator of a symmetric 2nd order tensor, 𝑗0 is the determinant of the jacobian matrix, 𝑗0 is the determinant of the jacobian matrix at time 0, σ is the true stress tensor, 𝐒 is the 2nd Piola- Kirchhoff stress tensor, 𝐂𝑆𝐸 is the material tangent modulus, 𝐂σ is the spatial tangent modulus and 𝑉𝑒 is the volume of the element. In the above, we have used various transformation formulae between different stress and constitutive tensors. At this point we are only interested in how to handle the stabilization portion of the strain rate field, the constant part is only used to update the midpoint stress as usual. Because of orthogonality properties of the involved matrices, it turns out that we may just insert the expression for the stabilization strain rate field to get 𝛿𝑊int 𝑠 ≈ ∫ 𝛿𝛆̃𝑠 ⎜⎛∫ ⎝ 𝑉𝑒 −T𝐂𝜎𝐉̂0 𝐉̂0 −1𝛆̇ ̃𝑠𝑑𝜏 ⎟⎞ 𝑑𝑉𝑝 ⎠ , (4.95a) = [𝛿𝐮̃𝑇 𝛿𝜶T] ∫ [ 𝚩̃𝑠(𝛏)𝑇 𝐆̃(𝛏)𝑇 ] ⎜⎛∫ ⎝ 𝑉𝑒 −T𝐂𝜎𝐉̂0 𝐉̂0 −1[𝚩̃𝑠(𝛏) 𝐆̃(𝛏)] [𝐮̇ 𝛂̇ ] 𝑑𝜏 ⎟⎞ 𝑑𝑉𝑝 ⎠ . (4.95b) The stabilization contribution to the internal force vector is given by [ 𝐟𝑢 𝐟𝛼 ] = [𝕵T ] ∫ [ 𝚩̃𝑠(𝛏)T 𝐆̃(𝛏)T ] ⎜⎛∫ ⎝ 𝑉𝑒 −T𝐂𝜎𝐉̂0 𝐉̂0 −1[𝚩̃𝑠(𝛏) 𝐆̃(𝛏)][𝕵 0 ][𝐮̇ 𝛂̇ ]𝑑𝜏 ⎟⎞ 𝑑𝑉𝑝 ⎠ . (4.96) In a discretization, the condition 𝐟𝛼 = 0 is used to determine Δ𝛂, the increment of the enhanced strain variables, from Δu, the increment in displacements. This is inserted back into the expression for the internal force vectors to determine 𝐟𝑢, the stabilization contribution to the internal force vector. The implementation of the element is very similar to the implementation of the one point integrated mean strain hexahedral by Flanagan and Belytschko [1981]. The hourglass forces are calculated in a different manner. From the midpoint stress update we get a bulk and shear modulus characterizing the material at this specific point in time. From this we form the isotropic spatial tangent modulus 𝐂𝛔 to be used for computing the stabilization force from Equation (4.96). 4.5 Fully Integrated Brick Elements and Mid-Step Strain Evaluation To avoid locking in the fully integrated brick elements strain increments at a point in a constant pressure, solid element are defined by [see Nagtegaal, Parks, anmmmmmd Rice 1974] 4-20 (Solid Elements) LS-DYNA Theory Manual Solid Elements Δ𝜀𝑥𝑥 = Δ𝜀𝑦𝑦 = ∂Δ𝑢 ∂𝑥𝑛+1 2⁄ ∂Δ𝑣 ∂𝑦𝑛+1 2⁄ Δ𝜀𝑧𝑧 = ∂Δ𝑤 ∂𝑧𝑛+1 2⁄ + 𝜙, Δ𝜀𝑥𝑦 = + 𝜙, Δ𝜀𝑦𝑧 = + 𝜙, Δ𝜀𝑧𝑥 = , , ∂Δ𝑣 ∂𝑥𝑛+1 2⁄ + ∂Δ𝑢 ∂𝑦𝑛+1 2⁄ ∂Δ𝑤 ∂𝑦𝑛+1 2⁄ ∂Δ𝑢 ∂𝑧𝑛+1 2⁄ + ∂Δ𝑣 ∂𝑧𝑛+1 2⁄ + ∂Δ𝑤 ∂𝑥𝑛+1 2⁄ , (4.97) where 𝜙 modifies the normal strains to ensure that the total volumetric strain increment at each integration point is identical 𝑛+1 2⁄ 𝜙 = Δ𝜀𝑣 ∂Δ𝑢 ∂𝑥𝑛+1 2⁄ + ∂Δ𝑣 ∂𝑦𝑛+1 2⁄ − + ∂Δ𝑤 ∂𝑧𝑛+1 2⁄ , 𝑛+1 2⁄ and Δ𝜀𝑣 is the average volumetric strain increment in the midpoint geometry ∫ 𝑣𝑛+1 2⁄ ⎜⎜⎛ ∂Δ𝑢 ∂𝑥𝑛+1 2⁄ ⎝ + ∂Δ𝑤 ∂𝑧𝑛+1 2⁄ ⎟⎟⎞ 𝑑𝑣𝑛+1 2⁄ ⎠ , + ∂Δ𝑣 ∂𝑦𝑛+1 2⁄ 𝑑𝑣𝑛+1 2⁄ ∫ 𝑣𝑛+1 2⁄ (4.98) (4.99) Δ𝑢,. Δ𝑣, and Δ𝑤 are displacement increments in the x, y, and z directions, respectively, and 𝑥𝑛+1 2⁄ = (𝑥𝑛 + 𝑥𝑛+1) , 𝑦𝑛+1 2⁄ = (𝑦𝑛 + 𝑦𝑛+1) , (4.100a) (4.100b) 2⁄ = 𝑧𝑛+1 (𝑧𝑛 + 𝑧𝑛+1) . To satisfy the condition that rigid body rotations cause zero straining, it is necessary to use the geometry at the mid-step in the evaluation of the strain increments. As the default, LS-DYNA currently uses the geometry at step 𝑛 + 1 to save operations; however, is always recommended, and, for explicit calculations, which involve rotating parts, the mid-step geometry should be used especially if the number of revolutions is large. The mid-step geometry can be activated either globally or for a subset of parts in the model by using the options on the control card, *CONTROL_ACCURACY. the mid-step strain calculation implicit calculations (4.100c) for Solid Elements LS-DYNA Theory Manual Figure 4.4. Four node tetrahedron. Since the bulk modulus is constant in the plastic and viscoelastic material models, constant pressure solid elements result. In the thermoelastoplastic material, a constant temperature is assumed over the element. In the soil and crushable foam material, an average relative volume is computed for the element at time step 𝑛 + 1, and the pressure and bulk modulus associated with this relative volume is used at each integration point. For equations of state, one pressure evaluation is done per element and is added to the deviatoric stress tensor at each integration point. The foregoing procedure requires the strain-displacement matrix corresponding to Equations (4.66) and consistent with a constant volumetric strain, 𝐁̅̅̅̅̅, be used in the nodal force calculations [Hughes 1980]. It is easy to show that: that 𝐅 = ∫ (𝐁̅̅̅̅̅𝑛+1) 𝑣𝑛+1 𝛔𝑛+1𝑑𝑣 = ∫ (𝐁𝑛+1) 𝑣𝑛+1 𝛔𝑛+1𝑑𝑣, (4.101) and avoid the needless complexities of computing 𝐁̅̅̅̅̅. 4.6 Four Node Tetrahedron Element The four node tetrahedron element with one point integration, shown in Figure 4.4, is a simple, fast, solid element that has proven to be very useful in modeling low density foams that have high compressibility. For most applications, however, this element is too stiff to give reliable results and is primarily used for transitions in meshes. The formulation follows the formulation for the one point solid element with the difference that there are no kinematic modes, so hourglass control is not needed. The basis functions are given by: 𝑁1(𝑟, 𝑠, 𝑡) = 𝑟, 𝑁2(𝑟, 𝑠, 𝑡) = 𝑠, 4-22 (Solid Elements) (4.102a) LS-DYNA Theory Manual Solid Elements 𝑁3(𝑟, 𝑠, 𝑡) = 1 − 𝑟 − 𝑠 − 𝑡, 𝑁4(𝑟, 𝑠, 𝑡) = 𝑡. (4.102c) (4.102d) If a tetrahedron element is needed, this element should be used instead of the collapsed solid element since it is, in general, considerably more stable in addition to being much faster. Automatic sorting can be used, see *CONTROL_SOLID keyword, to segregate these elements in a mesh of 8 node solids for treatment as tetrahedrons. 4.7 Nodal Pressure Tetrahedron For applications requiring a tetrahedron mesh, the volume averaged tetrahedron type 13 is an interesting alternative to the standard single point tetrahedron, also known as the 1 point nodal pressure tetrahedron. The idea is to average the volumetric strain over adjacent elements to smooth the pressure response. To this end, we assume that 𝐸 is the set of all such elements in a model, and likewise 𝑁 is the set of all nodes belonging to these elements. We introduce the indicator 1/4 if node 𝑛 is connecting to element 𝑒 The volume of a node 𝑛 is defined as otherwise 𝑛 = { 𝜒𝑒 (4.103) 𝑛𝑉𝑒 (4.104) where 𝑉𝑒 is the exact volume of element 𝑒. This allows us to define an average jacobian 𝐽 ̅𝑒 for element 𝑒 as 𝑉𝑛 = ∑ 𝜒𝑒 𝑒∈𝐸 𝐽 ̅𝑒 = ∑ 𝜒𝑒 𝑛 { 𝑛∈𝑁 𝑉𝑛 0} 𝑉𝑛 (4.105) 0 is the nodal volume in the reference which is essentially the relative volume. Here 𝑉𝑛 configuration. The element is completely defined by the assumed deformation gradient given as 𝑭̅𝑒 = ( 1/3 𝐽 ̅𝑒 𝐽𝑒 ) 𝑭𝑒 (4.106) where 𝑭𝑒 is the deformation gradient from the isoparametric shape functions and 𝐽𝑒 = det𝑭𝑒, also given as 𝐽𝑒 = 𝑉𝑒 0. 𝑉𝑒 (4.107) The assumed rate of deformation, derived from 𝑭̅𝑒, is given as 𝛿𝐽𝑒 𝐽𝑒 meaning that the volumetric strain is replaced by that of the averaged one. Continuing, the virtual work equation is given as ) 𝑰 + 𝛿𝑭𝑒𝑭𝑒 𝛿𝜺̅𝑒 = −1 (4.108) − ( 𝛿𝐽 ̅𝑒 𝐽 ̅𝑒 LS-DYNA Draft ∑ 𝒇𝑛 𝑛∈𝑁 𝑇𝛿𝒙𝑛 = ∑ 𝝈𝑒: 𝛿𝜺̅𝑒𝐽𝑒𝑉𝑒 𝑒∈𝐸 Solid Elements LS-DYNA Theory Manual Figure 4.5. Six node Pentahedron. which provides the equation for the nodal forces, 𝒇𝑛. An expression for the strain- 𝑛, is deduced from combining (4.108) and the relation 𝛿𝜺̅𝑒 = displacement matrix, 𝑩𝑒 ∑ 𝑩𝑒 𝑛∈𝑁 . It turns out to be given as 𝑛𝛿𝒙𝑛 𝑛 and 𝑩̃𝑒 𝑛 = ∑ ∑ 𝜒𝑓 𝑩𝑒 𝑓 ∈𝐸 𝑚 𝑉𝑓 𝜒𝑒 𝐽 ̅𝑒𝑉𝑚 𝑛 are the volumetric and deviatoric parts of the standard (derived from where 𝑩̅̅̅̅̅𝑒 isoparametric shape functions) strain displacement matrix. Noticable is that the support for the assumed strain displacement is not restricted to the nodal connectivity of a single element but is spread over a region of adjacent elements. This renders a less sparse stiffness matrix, but also explains the smoothening effect of the pressure. 𝑛 + 𝑩̃𝑒 𝑩̅̅̅̅̅𝑓 𝑚∈𝑁 (4.110) 4.8 Six Node Pentahedron Element The pentahedron element with two point Gauss integration along its length, shown in Figure 4.5, is a solid element that has proven to be very useful in modeling axisymmetric structures where wedge shaped elements are used along the axis-of- revolution. The formulation follows the formulation for the one point solid element with the difference that, like the tetrahedron element, there are no kinematic modes, so hourglass control is not needed. The basis functions are given by: 𝑁1(𝑟, 𝑠, 𝑡) = 𝑁2(𝑟, 𝑠, 𝑡) = (1 − 𝑡)𝑟, (1 − 𝑡)(1 − 𝑟 − 𝑠), (4.111a) (4.111b) LS-DYNA Theory Manual Solid Elements 15 16 17 20 13 11 12 19 14 18 10 DOF ui, vi, wi DOF ui, vi, wi, θ xi, θ yi, θ zi Figure 4.6. The 20-node solid element is transformed to an 8-node solid with 6 degrees-of-freedom per node. 𝑁3(𝑟, 𝑠, 𝑡) = 𝑁4(𝑟, 𝑠, 𝑡) = 𝑁5(𝑟, 𝑠, 𝑡) = 𝑁6(𝑟, 𝑠, 𝑡) = (1 + 𝑡)(1 − 𝑟 − 𝑠), (1 + 𝑡)𝑟, (1 − 𝑡)𝑠, (1 + 𝑡)𝑠. (4.111c) (4.111d) (4.111e) (4.111f) If a pentahedron element is needed, this element should be used instead of the collapsed solid element since it is, in general, more stable and significantly faster. Automatic sorting can be used, see *CONTROL_SOLID keyword, to segregate these elements in a mesh of 8 node solids for treatment as pentahedrons. Selective-reduced integration is used to prevent volumetric locking, i.e., a constant pressure over the domain of the element is assumed. 4.9 Fully Integrated Brick Element With 48 Degrees-of- Freedom The forty-eight degree of freedom brick element is derived from the twenty node solid element; see Figure 4.6, through a transformation of the nodal displacements and rotations of the mid-side nodes [Yunus, Pawlak, and Cook, 1989]. This element has the Solid Elements LS-DYNA Theory Manual Figure 4.7. A typical element edge is shown from [Yunus, Pawlak, and Cook, 1989]. advantage that shell nodes can be shared with brick nodes and that the faces have just four nodes — a real advantage for the contact-impact logic. The accuracy of this element is relatively good for problems in linear elasticity but degrades as Poisson’s ratio approaches the incompressible limit. This can be remedied by using incompatible modes in the element formulation, but such an approach seems impractical for explicit computations. The instantaneous velocity for a midside node 𝑘 is given as a function of the corner node velocities as , (𝑢̇𝑖 + 𝑢̇𝑗) + (𝑣̇𝑖 + 𝑣̇𝑗) + 𝑢̇𝑘 = 𝑣̇𝑘 = 𝑤̇ 𝑘 = 𝑦𝑗 − 𝑦𝑖 𝑧𝑗 − 𝑧𝑖 𝑥𝑗 − 𝑥𝑖 𝑧𝑗 − 𝑧𝑖 𝑥𝑗 − 𝑥𝑖 𝑦𝑗 − 𝑦𝑖 (𝑤̇ 𝑖 + 𝑤̇ 𝑗) + (𝜃̇ 𝑦𝑗 − 𝜃̇ 𝑦𝑖) + (𝜃̇ 𝑥𝑖 − 𝜃̇ 𝑥𝑗), (𝜃̇ 𝑧𝑗 − 𝜃̇ 𝑧𝑖) + (𝜃̇ 𝑦𝑖 − 𝜃̇ 𝑦𝑗), (𝜃̇ 𝑥𝑗 − 𝜃̇ 𝑥𝑖) + (𝜃̇ 𝑧𝑖 − 𝜃̇ 𝑧𝑗), (4.112) where 𝑢, 𝑣, 𝑤, 𝜃𝑥, 𝜃𝑦, and 𝜃z are the translational and rotational displacements in the global 𝑥, 𝑦, and 𝑧 directions. The velocity field for the twenty-node hexahedron element in terms of the nodal velocities is: {⎧𝑢̇ }⎫ 𝑣̇ 𝑤̇ ⎭}⎬ ⎩{⎨ = 𝜙1 𝜙2 … 𝜙20 ⎡ 0 … 0 ⎢ 0 … 0 ⎣ 0 … 0 𝜙1 𝜙2 … 𝜙20 0 … 0 0 … 0 ⎤ 0 … 0 ⎥ 𝜙1 𝜙2 … 𝜙20⎦ ⎧ 𝑢̇1 ⎫ }}} {{{ ⋮ 𝑢̇20 }}} {{{ 𝑣̇1 } { ⋮ ⎬ ⎨ }}}} {{{{ 𝑣̇20 𝑤̇ 1 }}} {{{ ⋮ 𝑤̇ 20⎭ ⎩ , (4.113) where 𝜙𝑖 are given by [Bathe and Wilson 1976] as, LS-DYNA Theory Manual Solid Elements DOF ui, vi, wi DOF ui, vi, wi, θ xi, θ yi, θ zi Figure 4.8. Twenty-four degrees of freedom tetrahedron element [Yunus, Pawlak, and Cook, 1989]. 𝜙1 = 𝑔1 − 𝜙2 = 𝑔2 − 𝜙3 = 𝑔3 − , (𝑔9 + 𝑔12 + 𝑔17) (𝑔9 + 𝑔10 + 𝑔18) , (𝑔10 + 𝑔11 + 𝑔19) (𝑔11 + 𝑔12 + 𝑔20) 𝜙5 = 𝑔5 − 𝜙6 = 𝑔6 − , 𝜙7 = 𝑔7 − 𝜙8 = 𝑔8 − , (𝑔13 + 𝑔16 + 𝑔17) (𝑔13 + 𝑔14 + 𝑔18) , (𝑔14 + 𝑔15 + 𝑔19) (𝑔15 + 𝑔16 + 𝑔20) , , 𝜙4 = 𝑔4 − 𝜙𝑖 = 𝑔𝑖 for 𝑗 = 9, … , 20 𝑔𝑖 = 𝐺(𝜉 , 𝜉𝑖)𝐺(𝜂, 𝜂𝑖)𝐺(𝜁 , 𝜁𝑖), , 𝐺(𝛽, 𝛽𝑖) = {⎧1 ⎩{⎨ (1 + 𝛽𝛽𝑖) 1 − 𝛽2 for, 𝛽𝑖 = ±1; 𝛽 = 𝜉 , 𝜂, 𝜁 . for, 𝛽𝑖 = 0 (4.114) The standard formulation for the twenty node solid element is used with the above trans-formations. The element is integrated with a fourteen point integration rule [Cook 1974]: 1 1 1 −1 −1 ∫ ∫ ∫ 𝑓 (𝜉 , 𝜂 , 𝜁 )𝑑𝜉𝑑𝜂𝑑𝜁 = −1 𝐵6 [𝑓 (−𝑏, 0,0) + 𝑓 (𝑏, 0,0) + 𝑓 (0, −𝑏, 0) + ⋯ + (6 terms)] + 𝐶8 [𝑓 (−𝑐, −𝑐, −𝑐) + 𝑓 (𝑐, −𝑐, −𝑐) + 𝑓 (𝑐, 𝑐, −𝑐) + ⋯ + (8 terms)], where 𝐵6 = 0.8864265927977938, 𝐶8 = 0.3351800554016621, 𝑏 = 0.7958224257542215, 𝑐 = 0.7587869106393281. (4.115) (4.116) Solid Elements LS-DYNA Theory Manual Cook reports that this rule has nearly the same accuracy as the twenty-seven point Gauss rule, which is very costly. The difference in cost between eight point and fourteen point integration, though significant, is necessary to eliminate the zero energy modes. 4.10 Fully Integrated Tetrahedron Element With 24 Degrees- of-Freedom The twenty-four degree of freedom tetrahedron element is derived from the ten- node tetrahedron element; see Figure 4.8, following the same procedure used above for the forty-eight degree of freedom brick element [Yunus, Pawlak, and Cook, 1989]. This element has the advantage that shell nodes can be shared with its nodes and it is compatible with the brick element discussed above. The accuracy of this element is relatively good-at least when compared to the constant strain tetrahedron element. This is illustrated by the bar impact example in Figure 4.9 which compares the 12 and 24 degree of freedom tetrahedron elements. The 12 degree-of-freedom tetrahedron displays severe volumetric locking. In our implementation we have not strictly followed the reference. In order to prevent locking in applications that involve incompressible behavior, selective reduced integration is used with a total of 5 integration points. Although this is rather expensive, no zero energy modes exist. We use the same approach in determining the rotary mass that is used in the implementation of the shell elements. LS-DYNA Theory Manual Solid Elements Figure 4.9. A comparison of the 12 and 24 degree-of-freedom tetrahedron elements is shown. The 12 degree-of-freedom tetrahedron element on the top displays severe volumetric locking. Solid Elements LS-DYNA Theory Manual Figure 4.10a. Construction of a hexahedron element with five tetrahedrons. Figure 4. 10b. Construction of a hexahedron element with six tetrahedrons Figures 4.10a and 4. 10b show the construction of a hexahedron element from five and six tetrahedron elements, respectively. When two sides of the adjacent bricks made from five tetrahedrons are together, it is likely that four unique triangular segments exist. This creates a problem in LS-PREPOST, which uses the numbering as a basis for eliminating interior polygons prior to display. Consequently, the graphics in the post-processing phase can be considerably slower with the degeneration in Figure 4.10a. However, marginally better results may be obtained with five tetrahedrons per hexahedron due to a better constraint count. LS-DYNA Theory Manual Solid Elements 4.11 The Cosserat Point Elements in LS-DYNA 4.11.1 Introduction The Cosserat Point Elements (CPE) are based on the works by Jabareen et.al.[1,2]. In contrast with a conventional approach, the CPE is treated as a structure rather than a continuum. The kinematic variables of the CPE are characterized by a volume averaged deformation gradient and other measures of inhomogeneous deformations. The CPE models the response of a simple continuum (not a generalized Cosserat media) and the additional kinematic degrees of freedom model physical modes of deformation of the structure. Moreover, the CPE uses a hyperelastic constitutive equation for elastic response with the strain energy of the CPE being separated additively into a part dependent on the strain energy of the three-dimensional material and another strain energy associated with inhomogeneous deformations. Also, for the tetrahedral CPE use is made of a new measure of dilatation that stabilizes hourglass type modes in large deformations. This formulation is valid for large deformations and the coefficients in the inhomogeneous strain energy are ingeniously determined by comparison with exact linear solutions. This ensures that CPE yields accurate results for elementary deformation modes in linear elasticity. Moreover, using the average deformation gradient for the response to homogeneous deformations the CPE formulation can be coupled with arbitrary material models in LS-DYNA. Still the element is, due to its complexity and slight loss of generality, first and foremost recommended for hyperelasticy in implicit analysis. Section 4.11.2 through 4.11.8 describes the theory for the hexahedral CPE element, the tetrahedron is based on the same concepts except for the volumetric correction presented in Section 4.11.5. For more details we refer to [1] and [2]. We end with two examples in Sections 4.11.9 and 4.11.10. D3 D1 D2 d3 d1 d2 Figure 4.11. The CPE hexahedron Solid Elements 4.11.2 Geometry LS-DYNA Theory Manual The geometry of the hexahedral CPE element is characterized by the three-dimensional directors 𝐃𝑖 and 𝐝𝑖, 𝑖 = 0,1, … ,7, where the formers are associated with the reference configuration and the latters with the current configuration. The reciprocal vectors 𝐃𝑖 and 𝐝𝑖, 𝑖 = 1,2,3, are such that 𝑗, 𝐝𝑖 ⋅ 𝐝𝑗 = 𝐃𝑖 ⋅ 𝐃𝑗 = 𝛿𝑖 𝑖, 𝑗 = 1, 2, 3, and we also have that The coordinates 𝜃𝑖, 𝑖 = 1,2,3, ranges between |𝐃𝑖| = 1, 𝑖 = 1, 2, 3, (4.11.117) (4.11.118) −𝐻/2 ≤ 𝜃1 ≤ 𝐻/2, − 𝑊/2 ≤ 𝜃2 ≤ 𝑊/2, − 𝐿/2 ≤ 𝜃3 ≤ 𝐿/2, (4.11.119) and the 𝐀 matrix is given such that 𝐃𝑖 = ∑ 𝐴𝑖 𝑗𝐗𝑗 , 𝐝𝑖 = ∑ 𝐴𝑖 𝑗𝐱𝑗 , 𝑖 = 0, 1, . . . , 7, (4.11.120) 𝑗=0 𝑗=0 where 𝐗𝑖 and 𝐱𝑖 are the nodal coordinates in the reference and current configuration, respectively. Hence the 𝐀 matrix represents the mapping between the nodal coordinates and the Cosserat point directors. The reference position vector 𝐗 is expressed as 𝐗 = 𝐗(𝜃1, 𝜃2, 𝜃3) = ∑ 𝑁𝑗(𝜃1, 𝜃2, 𝜃3)𝐃𝑗 , (4.11.121) 𝑗=0 and likewise the current position 𝐱 as 𝐱 = 𝐱(𝜃1, 𝜃2, 𝜃3) = ∑ 𝑁𝑗(𝜃1, 𝜃2, 𝜃3)𝐝𝑗, 𝑗=0 The shape functions are given as 𝑁0 = 1, 𝑁4 = 𝜃1𝜃2, 𝑁5 = 𝜃1𝜃3, 𝑁6 = 𝜃2𝜃3, 𝑁7 = 𝜃1𝜃2𝜃3. 𝑁3 = 𝜃3, 𝑁1 = 𝜃1, 𝑁2 = 𝜃2, (4.11.122) (4.11.123) 4.11.3 Deformation and strain The deformation measures used are 𝐅 = ∑ 𝐝𝑖 ⊗ 𝐃𝑖 𝑖=1 , 𝛃𝑖 = 𝐅−1𝐝𝑖+3 − 𝐃𝑖+3 (𝑖 = 1,2,3,4), 𝐅̅̅̅̅ = 𝐅 (𝐈 + ∑ 𝛃𝑖 ⊗ 𝐕𝑖 ), (4.11.124) 𝑖=1 where 𝐅̅̅̅̅ is the volume averaged deformation gradient and thus represents the inhomogeneous homogeneous deformations whereas 𝛃𝑖 are measures of deformations. As for the 𝐕𝑖 we have the LS-DYNA Theory Manual Solid Elements 𝑉 = 𝐻𝑊𝐿 (𝐃1 × 𝐃2 ⋅ 𝐃3 + 𝐻2 12 𝐃4 × 𝐃5 ⋅ 𝐃1 + × 𝐃4 ⋅ 𝐃2 + 𝐃6 𝑊2 12 𝐿2 12 𝐃5 × 𝐃6 ⋅ 𝐃3) , 𝐃2 × 𝐃6) , (4.11.125) 𝐕1 = 𝑉−1𝐻𝑊𝐿 ( 𝐕2 = 𝑉−1𝐻𝑊𝐿 ( 𝐕3 = 𝑉−1𝐻𝑊𝐿 ( 𝐕4 = 𝟎, 𝐻2 12 𝐻2 12 𝑊2 12 𝐃5 × 𝐃1 + 𝐃1 × 𝐃4 + 𝐃4 × 𝐃2 + 𝑊2 12 𝐿2 12 𝐿2 12 𝐃6 × 𝐃3) , 𝐃3 × 𝐃5) , The velocity gradient consistent with 𝐅̅̅̅̅ is given as 𝐋̅ = 𝐅̅̅̅̅̇𝐅̅̅̅̅−1 = 𝐋 + ∑(𝐝̇ 𝑗+3 − 𝐋𝐝𝑗+3) ⊗ 𝐕𝑗 𝐅̅̅̅̅−1, 𝑗=1 (4.11.126) where 𝐋 = 𝐅̇𝐅−1, which in turn gives the rate –of-deformation and spin tensors as ̇ = 𝛆̅ (𝐋̅ + 𝐋̅ 𝑇), 𝛚̅̅̅̅̅̅ = (𝐋̅ − 𝐋̅ 𝑇). (4.11.127) 4.11.4 Stress and Force On the other hand, 𝐋 = ∑ 𝐝̇ 𝑖=1 𝑖 ⊗ 𝐝𝑖 , (4.11.128) so we can rewrite 𝐋̅ as 𝐋̅ = ∑ 𝐝̇ 𝑖=1 𝑖 ⊗ 𝐝𝑖 ⎜⎛𝐅̅̅̅̅ − ∑ 𝐝𝑗+3 ⊗ 𝐕𝑗 ⎝ 𝑗=1 ⎟⎞ 𝐅̅̅̅̅−1 + ∑ 𝐝̇ ⎠ 𝑖=1 The Cauchy stress is given by the constitutive law or for the hyperelastic case 𝛔∇ = 𝐟hypo(𝛆̅ ̇, . . . ), 𝛔 = 𝐟hyper(𝐅̅̅̅̅, . . . ), so the nonzero internal force vectors are given as 𝑖+3 ⊗ 𝐕𝑖 𝐅̅̅̅̅−1. (4.11.129) (4.11.130) (4.11.131) Solid Elements LS-DYNA Theory Manual 𝑖 = 𝐽 ̅𝑉𝛔𝐅̅̅̅̅−𝑇 𝐭𝜎 ⎜⎛𝐅̅̅̅̅𝑇 − ∑ 𝐕𝑗 ⊗ 𝐝𝑗+3 ⎝ 𝑗=1 ⎟⎞ 𝐝𝑖, ⎠ 𝑖+3 = 𝑉𝛔𝐅̅̅̅̅−𝑇𝐕𝑖, 𝐭𝜎 𝑖 = 1, 2, 3. (4.11.132) The first expression above can in turn be rewritten as 𝑖 = 𝐭𝜎 ⎜⎛𝐽 ̅𝑉𝛔 − ∑ 𝐭𝜎 ⎝ 𝑗=1 𝑗+3 ⊗ 𝐝𝑗+3 ⎟⎞ 𝐝𝑖, ⎠ 𝑖 = 1, 2, 3. (4.11.133) 4.11.5 CPE3D10 modification For the 10-noded tetrahedron, a modified deformation gradient is used in the constitutive law, given by 𝐅̃ = (𝐽 ̃ 𝐽 ̅⁄ ) 1/3 𝐅̅̅̅̅, meaning it has been modified for the volumetric response. Here This gives a consistent velocity gradient as 𝐽 ̃ = 𝐽 ̅ + 𝜂𝐽, 𝐋̃ = 𝐋̅ + ⎜⎛𝜂̇ + 𝜂 𝐽 ̃⎝ {⎧𝐽 ̇ ⎩{⎨ − 𝐽 ̅ }⎫ 𝐽 ̅⎭}⎬ ⎟⎞ 𝐈. ⎠ The Cauchy stress is now given by the constitutive law 𝛔∇ = 𝐟hypo(𝛆̃ ̇, … ), ̇ = 𝛆̃ (𝐋̃ + 𝐋̃ 𝑇), or for the hyperelastic case 𝛔 = 𝐟hyper(𝐅̃, . . . ), (4.11.134) (4.11.135) (4.11.136) (4.11.137) (4.11.138) and the corresponding internal force can be identified through a principle of virtual work ∑ 𝐭𝜎 𝑖=0 𝑖 ⋅ 𝐝̇ = 𝐽 ̃𝑉𝐋̃ ⋅ 𝛔. For the hyperelastic special case we have 𝛔 = ∂Σ ∂𝐽 ̃ 𝐈 + 2𝐽 ̃−1 [𝐅̅̅̅̅′ ∂Σ ∂𝐂̅′ 𝐅̅̅̅̅′𝑇 − ( ∂Σ ∂𝐂̅′ ⋅ 𝐂̅′) 𝐈], and since (4.11.139) (4.11.140) 4-34 (Solid Elements) LS-DYNA Theory Manual Solid Elements 𝐋̃ = ∑ 𝐝̇ 𝑖=1 𝑖 ⊗ 𝐝𝑖 + + ⎟⎞ 𝐅̅̅̅̅−1 + ∑ 𝐝̇ ⎠ ((𝐝𝑘) 𝑖=1 𝐝̇ 𝑗=1 ∑ ∑ 𝑗=1 𝑘=1 ⎜⎛𝐅̅̅̅̅ − ∑ 𝐝𝑗+3 ⊗ 𝐕𝑗 ⎝ 𝐽 ̃ ⎡𝜂 ⎢ 𝐽 ̃⎣ ⎜⎛∑ ∑ 𝐝𝑖 ⋅ 𝐝𝑗+3𝐝̇ ⎝ ⎡ ∂𝜂 ⎢ ∂𝑏𝑗 ⎣ 𝑗=1 𝑖=1 𝑖=1 𝑖 ⋅ 𝐅̅̅̅̅−𝑇𝐕𝑗 − 𝑗+3 − ∑ 𝐝𝑖 ⋅ 𝐝𝑗+3𝐝𝑘 ⋅ 𝐝̇ ) ⎤ ⎥ ⎦ (4.11.141) ∑ 𝐝̇ 𝑖=1 𝑖+3 ⋅ 𝐅̅̅̅̅−𝑇𝐕𝑖 ⎟⎞ ⎠ ⎤ 𝐈, ⎥ ⎦ 𝑖+3 ⊗ 𝐕𝑖 𝐅̅̅̅̅−1 putting back these expressions into the virtual work expression above and adding the hourglass internal forces from below we get the same as in [2]. 4.11.6 Hourglass The hourglass resistance is based on a strain energy potential given as 𝜓 = 𝑉𝜇 12(1 − 𝜈) ∑ ∑ ∑ ∑ 𝑏𝑖 𝑖=1 𝑘=1 𝑗=1 𝑙=1 𝑗𝐵𝑗𝑙 𝑖𝑘𝑏𝑘 , (4.11.142) where the inhomogeneous (hourglass) strain quantities are defined as 𝑗 = 𝛃𝑖 ⋅ 𝐃𝑗, 𝑏𝑖 𝑖 = 1, 2, 3, 4, 𝑗 = 1, 2, 3, (4.11.143) and the constant symmetric matrix 𝐁 contains geometry and constitutive information for obtaining accurate results for small deformations. Furthermore, 𝜇 represents the shear modulus of the material and 𝜈 is the Poisson’s ratio. The hourglass force is then given as ⎜⎛∂𝑏𝑗 ⎟⎞ ∂𝐝𝑖⎠ ⎝ Differentiating the strain quantities results in = ∑ ∑ 𝑗=1 𝑘=1 ∂𝜓 ∂𝑏𝑗 𝑖 = ( 𝐭ℎ ∂𝜓 ∂𝐝𝑖 ) , 𝑖 = 0, 1, … ,7. (4.11.144) ∂𝑏𝑗 ∂𝐝𝑖 ∂𝑏𝑗 ∂𝐝𝑖+3 = −𝐝𝑖 ⋅ 𝐝𝑗+3(𝐝𝑘) , 𝑖 = 1, 2, 3 𝑗(𝐝𝑘) = 𝛿𝑖 , 𝑖 = 1,2,3,4 (4.11.145) which inserted into the expression for the force yields Solid Elements LS-DYNA Theory Manual 𝑖 = − 𝐭ℎ 𝑗+3 ⊗ 𝐝𝑗+3 ⎜⎛∑ 𝐭ℎ ⎝ 𝑗=1 ∂𝜓 𝑗 𝐝𝑗 ∂𝑏𝑖 𝑖+3 = ∑ 𝐭ℎ 𝑗=1 , 𝑖 = 1,2,3,4 ⎟⎞ 𝐝𝑖, ⎠ 𝑖 = 1,2,3 (4.11.146) 4.11.7 Comparison to Jabareen & Rubin Putting the material and hourglass force together yields 𝐭𝑖 = 𝐭𝜎 𝑖 = 0,1, . . . ,7, 𝑖 , 𝑖 + 𝐭ℎ hence 𝐭𝑖 = ⎜⎛𝐽 ̅𝑉𝛔 − ∑ 𝐭𝑗+3 ⊗ 𝐝𝑗+3 ⎝ 𝑗=1 𝐭𝑖+3 = 𝐽 ̅𝑉𝛔𝐅̅̅̅̅−T𝐕𝑖 + ∑ 𝑗=1 𝑗 𝐝𝑗 ∂𝜓 ∂𝑏𝑖 ⎟⎞ 𝐝𝑖 ⎠ 𝑖 = 1,2,3 𝑖 = 1,2,3,4 (4.11.147) (4.11.148) 𝑗 are augmented with the geometry parameters 𝐻,𝑊 and 𝐿, In [1], the hourglass strains 𝑏𝑖 whereas here we have merged this information into the constitutive matrix 𝐁 for the purpose of simplifying the presentation. In [1] a hyperelastic constitutive law is assumed with a strain energy potential Σ = Σ(𝐂̅) and the Cauchy stress is then given as 𝛔 = 2𝐽 ̅−1𝐅̅̅̅̅ ∂Σ ∂𝐂̅ 𝐅̅̅̅̅T. (4.11.149) Taking all this into account, and consulting (2.13-2.14) in [1], the implemented CPE element in LS-DYNA should be consistent with the theory. 4.11.8 Nodal formulation To be of use in LS-DYNA, the CPE element has to be formulated in terms of the nodal variables, meaning that the internal forces that are conjugate to 𝐱̇𝑖, 𝑖 = 0,1, . . . ,7, with respect to internal energy rate are given as 𝑖𝐭𝑗 𝐟𝑖 = ∑ 𝐴𝑗 𝑗=0 , 𝑖 = 0,1, … ,7. (4.11.150) LS-DYNA Theory Manual Solid Elements Figure 4.11. Stress profile for tip loading in two directions for various mesh densities and distortions 4.11.9 Cantilever Beam Example First a mesh distortion test for small deformations where a cantilever beam with various mesh densities and distortions were simulated. The stress profiles for loading in two directions are shown in Figure 4.11. The tip displacements were monitored and compared to the analytical solution, and the results for the CPE element is very promising as is shown in figure below and Table 4.11 when compared to the Belytschko-Bindeman and Puso element [3,4]. 0.7 0.6 0.5 0.4 0.3 0.2 0.1 0 CPE B-B Puso 0.2 0.4 0.6 Mesh size 0.8 1 Figure 4.11. Mesh convergence rate for different element formulations Solid Elements LS-DYNA Theory Manual Cosserat Belytschko-Bindeman 1.7% 0.8% 0.6% 0.3% 0.2% 0.2% 0.1% 0.1% 0.1% 0.1% 61.8% 46.8% 40.0% 39.8% 33.9% 27.0% 24.6% 22.3% 19.0% 15.4% Puso 24.8% 14.7% 14.5% 9.2% 8.5% 6.2% 5.3% 3.6% 0.9% 0.3% Table 4.11. Comparison to analytical solution for tip loading 4.11.10 Compression Test for Rubber Example The second example is a plane strain deformation of an incompressible rubber block on a frictionless surface when partially loaded by a rigid plate. The block is modeled with quadratic tetrahedrons and a large deformation formulation applies. Five different mesh topologies are investigated for two different element formulations (CPE and full integration) where the orientation of the tetrahedral elements is different in each mesh whereas the mesh density is kept constant. The outer edges of the block for the different meshes are depicted in the figure above and indicate once again that the CPE element formulation is relatively insensitive to the mesh. Figure 4.11. Insensitivity illustration of the 10-noded CPE tetrahedron 4.11.11 References [1]M. Jabareen and M.B. Rubin, A Generalized Cosserat Point Element (CPE) for Isotropic Nonlinear Elastic Materials including Irregular 3-D Brick and Thin Structures, J. Mech. Mat. Struct. 3-8, pp. 1465-1498, 2008. [2]M. Jabareen, E. Hanukah and M.B. Rubin, A Ten Node Tetrahedral Cosserat Point Element (CPE) for Nonlinear Isotropic Elastic Materials. Comput Mech 52, pp 257-285, 2013. LS-DYNA Theory Manual Solid Elements Figure 4.11. The contour S encloses an area A. [3]M.A. Puso, A Highly Efficient Enhanced Assumed Strain Physically Stabilized Hexahedral Element, In. J. Num. Methods. Eng 49-8, pp. 1029-1064, 2000. [4]T. Belytschko and L.P. Bindeman , Assumed Strain Stabilization of the Eight Node Hexahedral Element, Comp. Methods Appl. Mech. Eng. 105-2, pp. 225- 260, 1993. 4.12 Integral Difference Scheme as Basis For 2D Solids Two dimensional solid element in LS-DYNA include: • Plane stress 2D element • Plane strain 2D shell element • Axisymmetric 2D Petrov-Galerkin (area weighted) element • Axisymmetric 2D Galerkin (volume weighted) element These elements have their origins in the integral difference method of Noh [1964] which is also used the HEMP code developed by Wilkins [1964, 1969]. In LS-DYNA, both two dimensional planar and axisymmetric geometries are defined in the 𝑥𝑦 plane. In axisymmetric geometry, however, the 𝑥 axis corresponds to the radial direction and the 𝑦 axis becomes the axis of symmetry. The integral difference method defines the components of the gradient of a function 𝐹 in terms of the line integral about the contour 𝑆 which encloses the area 𝐴: ∂𝐹 ∂𝑥 ∂𝐹 ∂𝑦 = lim A→0 = lim A→0 ∫ 𝐹(𝐧̂ ⋅ 𝐱̂)𝑑𝑆 |A| ∫ 𝐹(𝐧̂ ⋅ 𝐲̂)𝑑𝑆 . , |A| (4.151) Here, 𝐧̂ is the normal vector to 𝑆 and 𝐱̂ and 𝐲̂ are unit vectors in the x and y directions, respectively. See Figure 4.11. Solid Elements LS-DYNA Theory Manual strain rates nodal forces Figure 4.12. Strain rates are element centered and nodal forces are node centered. In this approach the velocity gradients which define the strain rates are element centered, and the velocities and nodal forces are node centered. See Figure 4.12. Noting that the normal vector 𝐧̂ is defined as: ∂𝑦 ∂𝑆 and referring to Figure 4.13, we can expand the numerator in equation (4.64): ∂𝑥 ∂𝑆 𝐧̂ = 𝐱̂ + 𝐲̂, ∫ 𝐹(n̂ ⋅ x̂)𝑑𝑆 = ∫ 𝐹 ∂𝑦 ∂𝑆 𝑑𝑆 = 𝐹23(𝑦3 − 𝑦2) + 𝐹34(𝑦4 − 𝑦3) + 𝐹41(𝑦1 − 𝑦4) + 𝐹12(𝑦2 − 𝑦1), where 𝐹𝑖𝑗 = (𝐹𝑖 + 𝐹𝑗)/2. (4.152) (4.153) Therefore, letting 𝐴 again be the enclosed area, the following expressions are obtained: ∂𝐹 ∂𝑥 = = 𝐹23(𝑦3 − 𝑦2) + 𝐹34(𝑦4 − 𝑦3) + 𝐹41(𝑦1 − 𝑦4) + 𝐹12(𝑦2 − 𝑦1) (𝐹2 − 𝐹4)(𝑦3 − 𝑦1) + (𝑦2 − 𝑦4)(𝐹3 − 𝐹1) . 2𝐴 Hence, the strain rates in the x and y directions become: ∂𝐹 ∂𝑥 = = 𝐹23(𝑦3 − 𝑦2) + 𝐹34(𝑦4 − 𝑦3) + 𝐹41(𝑦1 − 𝑦4) + 𝐹12(𝑦2 − 𝑦1) (𝐹2 − 𝐹4)(𝑦3 − 𝑦1) + (𝑦2 − 𝑦4)(𝐹3 − 𝐹1) , 2𝐴 (4.154) (4.155) LS-DYNA Theory Manual Solid Elements 1 Figure 4.13. Element numbering. and 𝜀𝑦𝑦 = ∂𝑦̇ ∂𝑦 = (𝑦̇2 − 𝑦̇4)(𝑥3 − 𝑥1) + (𝑥2 − 𝑥4)(𝑦̇3 − 𝑦̇1) 2𝐴 . The shear strain rate is given by: 𝜀𝑥𝑦 = ( ∂𝑦̇ ∂𝑥 + ∂𝑥̇ ∂𝑦 ), where ∂𝑦̇ ∂𝑥 ∂𝑥̇ ∂𝑦 = = (𝑦̇2 − 𝑦̇4)(𝑦3 − 𝑦1) + (𝑦2 − 𝑦4)(𝑦̇3 − 𝑦̇1) 2𝐴 (𝑥̇2 − 𝑥̇4)(𝑥3 − 𝑥1) + (𝑥2 − 𝑥4)(𝑥̇3 − 𝑥̇1) 2𝐴 . , (4.156) (4.157) (4.158) The zero energy modes, called hourglass modes, as in the three dimensional solid elements, can be a significant problem. Consider the velocity field given by: 𝑥̇3 = 𝑥̇1, 𝑥̇2 = 𝑥̇4, 𝑦̇3 = 𝑦̇1, and 𝑦̇2 = 𝑦̇4. As can be observed from Equations (4.97) and (4.98), 𝜀𝑥𝑥 = 𝜀𝑦𝑦 = 𝜀𝑥𝑦 = 0 and the element "hourglasses" irrespective of the element geometry. In the two-dimensional case, two modes exist versus twelve in three dimensions. The hourglass treatment for these modes is identical to the approach used for the shell elements, which are discussed later. In two-dimensional planar geometries for plane stress and plane strain, the finite element method and the integral finite difference method are identical. The velocity strains are computed for the finite element method from the equation: 𝛆̇ = 𝐁𝐯, (4.159) where 𝛆̇ is the velocity strain vector, B is the strain displacement matrix, and 𝐯 is the nodal velocity vector. Equation (4.100a) exactly computes the same velocity strains as the integral difference method if LS-DYNA Draft 𝐁 = 𝐁(𝑠, 𝑡)|𝑠=𝑡=0. Solid Elements LS-DYNA Theory Manual IV III II Figure 4.14. The finite difference stencil for computing nodal forces is shown. The update of the nodal forces also turns out to be identical. The momentum equations in two-dimensional planar problems are given by ( ( ∂𝜎𝑥𝑥 ∂𝑥 ∂𝜎𝑥𝑦 ∂𝑥 + + ∂𝜎𝑥𝑦 ∂𝑦 ∂𝜎𝑦𝑦 ∂𝑦 ) = 𝑥̈, ) = 𝑦̈. (4.161) Referring to Figure 4.14, the integral difference method gives Equation (4.113): ∂𝜎𝑥𝑥 ∂𝑥 = 𝜎𝑥𝑥1(𝑦𝐼 − 𝑦𝐼𝑉) + 𝜎𝑥𝑥2(𝑦𝐼𝐼 − 𝑦𝐼) + 𝜎𝑥𝑥3(𝑦𝐼𝐼𝐼 − 𝑦𝐼𝐼) + 𝜎𝑥𝑥4(𝑦𝐼𝑉 − 𝑦𝐼𝐼𝐼) (𝜌1𝐴1 + 𝜌2𝐴2 + 𝜌3𝐴3 + 𝜌4𝐴4) . (4.162) An element wise assembly of the discretized finite difference equations is possible leading to a finite element like finite difference program. This approach is used in the DYNA2D program by Hallquist [1980]. In axisymmetric geometries additional terms arise that do not appear in planar problems: ( ∂𝜎𝑥𝑥 ∂𝑥 ( + ∂𝜎𝑥𝑦 ∂𝑦 ∂𝜎𝑥𝑦 ∂𝑥 + + 𝜎𝑥𝑥 − 𝜎𝜃𝜃 ∂𝜎𝑥𝜃 + ∂𝜎𝑦𝑦 ∂𝑦 ) = 𝑥̈, ) = 𝑦̈, (4.163) where again note that 𝑦 is the axis of symmetry and 𝑥 is the radial direction. The only difference between finite element approach and the finite difference method is in the treatment of the terms, which arise from the assumption of axisymmetry. In the finite difference method the radial acceleration is found from the calculation: LS-DYNA Theory Manual Solid Elements 𝑥̈ = 𝜎𝑥𝑥1(𝑦𝐼 − 𝑦𝐼𝑉) + 𝜎𝑥𝑥2(𝑦𝐼𝐼 − 𝑦𝐼) + 𝜎𝑥𝑥3(𝑦𝐼𝐼𝐼 − 𝑦𝐼𝐼) + 𝜎𝑥𝑥4(𝑦𝐼𝑉 − 𝑦𝐼𝐼𝐼) [ (𝜌1𝐴1 + 𝜌2𝐴2 + 𝜌3𝐴3 + 𝜌4𝐴4) − 𝜎𝑥𝑦1(𝑥𝐼 − 𝑥𝐼𝑉) + 𝜎𝑥𝑦2(𝑥𝐼𝐼 − 𝑥𝐼) + 𝜎𝑥𝑦3(𝑥𝐼𝐼𝐼 − 𝑥𝐼𝐼) + 𝜎𝑥𝑦4(𝑥𝐼𝑉 − 𝑥𝐼𝐼𝐼) (𝜌1𝐴1 + 𝜌2𝐴2 + 𝜌3𝐴3 + 𝜌4𝐴4) ] + 𝛽, where 𝛽𝑓𝑒 is found by a summation over the four surrounding elements: 𝛽 = ∑ [ 𝑖=1 𝜎𝑥𝑥𝑖 − 𝜎𝜃𝜃𝑖 (𝜌𝑥)𝑖 ] . (4.164) (4.165) 𝑥𝑖 is the centroid of the ith element defined as the ratio of its volume 𝑉𝑖 and area 𝐴𝑖: 𝑉𝑖 𝐴𝑖 𝑥𝑖 = , (4.166) 𝜎𝜃𝜃𝑖 is the hoop stress, and 𝜌𝑖 is the current density. When applying the Petrov-Galerkin finite element approach, the weighting functions are divided by the radius, 𝑟: ∫ 𝛟T(∇ ⋅ 𝛔 + 𝐛 − 𝜌𝐮̈)𝑑𝑉 = ∫ 𝛟T(∇ ⋅ 𝛔 + 𝐛 − 𝜌𝐮̈)𝑑𝐴 = 0, (4.167) where the integration is over the current geometry. This is sometimes referred to as the "Area Galerkin" method. This approach leads to a time dependent mass vector. LS- DYNA also has an optional Galerkin axisymmetric element, which leads to a time independent mass vector. For structural analysis problems where pressures are low the Galerkin approach works best, but in problems of hydrodynamics where pressures are a large fraction of the elastic modulus, the Petrov-Galerkin approach is superior since the behavior along the axis of symmetry is correct. The Petrov-Galerkin approach leads to equations similar to finite differences. The radial acceleration is given by. 𝑥̈ = 𝜎𝑥𝑥1(𝑦𝐼 − 𝑦𝐼𝑉) + 𝜎𝑥𝑥2(𝑦𝐼𝐼 − 𝑦𝐼) + 𝜎𝑥𝑥3(𝑦𝐼𝐼𝐼 − 𝑦𝐼𝐼) + 𝜎𝑥𝑥4(𝑦𝐼𝑉 − 𝑦𝐼𝐼𝐼) [ (𝜌1𝐴1 + 𝜌2𝐴2 + 𝜌3𝐴3 + 𝜌4𝐴4) − 𝜎𝑥𝑦1(𝑥𝐼 − 𝑥𝐼𝑉) + 𝜎𝑥𝑦2(𝑥𝐼𝐼 − 𝑥𝐼) + 𝜎𝑥𝑦3(𝑥𝐼𝐼𝐼 − 𝑥𝐼𝐼) + 𝜎𝑥𝑦4(𝑥𝐼𝑉 − 𝑥𝐼𝐼𝐼) (𝜌1𝐴1 + 𝜌2𝐴2 + 𝜌3𝐴3 + 𝜌4𝐴4) ] + 𝛽𝑓𝑒, where 𝛽𝑓𝑒 is now area weighted. 𝛽𝑓𝑒 = 4(𝜌1𝐴1 + 𝜌2𝐴2 + 𝜌3𝐴3 + 𝜌4𝐴4) ∑ 𝑖=1 (𝜎𝑥𝑥𝑖 − 𝜎𝜃𝜃𝑖)𝐴𝑖 ⎢⎡ 𝑥𝑖 ⎣ ⎥⎤ . ⎦ (4.168) (4.169) In LS-DYNA, the two-dimensional solid elements share the same constitutive subroutines with the three-dimensional elements. The plane stress element calls the plane stress constitutive models for shells. Similarly, the plane strain and axisymmetric elements call the full three-dimensional constitutive models for solid elements. Slight Solid Elements LS-DYNA Theory Manual overheads exists since the strain rate components 𝜀̇𝑦𝑧 and 𝜀̇𝑧𝑥 are set to zero in the two- dimensional case prior to updating the six stress component; consequently, the additional work is related to having six stresses whereas only four are needed. A slowdown of LS-DYNA compared with DYNA2D of fifteen percent has been observed; however, some of the added cost is due to the internal and hourglass energy calculations, which were not done in DYNA2D. 4.12.1 Rezoning With 2D Solid Elements Lagrangian solution techniques generally function well for problems when element distortions are moderate. When distortions become excessive or when material breaks up, i.e., simply connected regions become multi-connected, these codes break down, and an Eulerian approach is a necessity. Between these two extremes, applications exist for which either approach may be appropriate but Lagrangian techniques are usually preferred for speed and accuracy. Rezoning may be used to extend the domain of application for Lagrangian codes. Rezoning capability was added to DYNA2D in 1980 and to LS-DYNA in version 940. In the current implementation the rezoning can be done interactively and used to relocate the nodal locations within and on the boundary of parts. This method is sometimes referred to as r-adaptive. The rezoning is accomplished in three steps listed below: 1. Generate nodal values for all variables to be remapped 2. Rezone one or more materials either interactively or automatically with command file. 3. Initialize remeshed regions by interpolating from nodal point values of old mesh. In the first step each variable is approximated globally by a summation over the number of nodal points 𝑛: 𝑔(𝑟, 𝑧) = ∑ 𝑔𝑖Φ𝑖(𝑟, 𝑧) 𝑖=1 , (4.170) where Φ𝑖 = set of piecewise continuous global basis functions 𝑔𝑖 = nodal point values Given a variable to be remapped h(𝑟, 𝑧), a least squares best fit is found by minimizing the functional 4-44 (Solid Elements) Π = ∫(𝑔 − ℎ)2𝑑𝐴, LS-DYNA Theory Manual Solid Elements Ajusted node Figure 4.15. The stencil used to relax an interior nodal point. i.e., 𝑑Π 𝑑𝑔𝑖 = 0, 𝑖 = 1, 2, … , 𝑛. This yields the set of matrix equations 𝐌𝐠 = 𝐟, where 𝐌 = ∑ 𝐌𝑒 = ∑ ∫ 𝚽𝚽T𝑑𝐴 , 𝐟 = ∑ 𝐟𝑒 = ∑ ∫ ℎ𝚽𝑑𝐴 . Lumping the mass makes the calculation of 𝑔 trivial , 𝑀𝑖 = ∑ 𝑀𝑖𝑗 𝑓𝑖 𝑀𝑖 𝑔𝑖 = . (4.172) (4.173) (4.174) (4.175) In step 2, the interactive rezoning phase permits: • Plotting of solution at current time • Deletion of elements and slidelines • Boundary modifications via dekinks, respacing nodes, etc. • Mesh smoothing A large number of interactive commands are available and are described in the Help package. Current results can be displayed by • Color fringes • Contour lines • Vectors plots Solid Elements LS-DYNA Theory Manual old mesh new mesh Figure 4.16. A four point Gauss quadrature rule over the new element is used to determine the new element centered value. • Principal stress lines • Deformed meshes and material outlines • Profile plots • Reaction forces • Interface pressures along 2D contact interfaces Three methods are available for smoothing: • Equipotential • Isoparametric • Combination of equipotential and isoparametric. In applying the relaxation, the new nodal positions are found and given by Equation (1.176) 𝑥 = 𝑦 = ∑ 𝜉𝑖𝑥𝑖 𝑖=1 ∑ 𝜉𝑖 𝑖=1 ∑ 𝜉𝑖𝑦𝑖 𝑖=1 ∑ 𝜉𝑖 𝑖=1 , , (4.176) where the nodal positions relative to the node being moved are shown in the sketch in Figure 4.15. LS-DYNA Theory Manual Solid Elements g3 g2 g4 g1 Figure 4.17. A four point Gauss quadrature rule over the new element is used to determine the new element centered value. The weights, 𝜉𝑖, for equipotential smoothing are 𝜉1 = 𝜉5 = [(𝑥7 − 𝑥3)2 + (𝑦7 − 𝑦3)2], 𝜉4 = 𝜉8 = −𝜉2, 𝜉2 = 𝜉6 = 𝜉3 = 𝜉7 = and are given by [(𝑥1 − 𝑥5)(𝑥7 − 𝑥3) + (𝑦1 − 𝑦5)(𝑦7 − 𝑦3)], [(𝑥1 − 𝑥5)2 + (𝑦1 − 𝑦5)2], 𝜉1 = 𝜉3 = 𝜉5 = 𝜉7 = .50, 𝜉2 = 𝜉4 = 𝜉6 = 𝜉8 = −.25, (4.177a) (4.177b) (4.177c) (4.177d) (4.178) for isoparametric smoothing. Since logical regularity is not assumed in the mesh, we construct the nodal stencil for each interior node and then relax it. The nodes are iteratively moved until convergence is obtained. In Chapter 14 of this manual, the smoothing procedures are discussed for three-dimensional applications. The new element centered values, ℎ∗, computed in Equation (1.179) are found by a 4 point Gauss Quadrature as illustrated in Figure 4.16. ℎ∗ = ∫ 𝑔𝑑𝐴 ∫ 𝑑𝐴 . (4.179) The Gauss point values are interpolated from the nodal values according to Equation (1.180). This is also illustrated by Figure 4.17. 𝑔𝑎 = ∑ 𝜙𝑖 (𝑠𝑎, 𝑡𝑎)𝑔𝑖. (4.180) LS-DYNA Theory Manual Cohesive Elements 5 Cohesive Elements The cohesive elements are used for modelling cohesive interfaces between faces of solid elements (types 19 and 21), faces of shell elements (types 20 and 22) and edges of shell elements (type ±29), typically for treating delamination. Element 19 𝒒3 Element 20 𝒒1 𝑛1 𝑚1 𝑛4 𝑚4 𝑛2 𝑚2 𝑛3 𝑚3 𝒒2 𝒒1 𝑛1 𝑚1 𝒒3 𝑛4 𝑛2 𝑚4 𝑛3 𝑚2 𝑚3 𝒒2 Element ±29 𝑡 𝒒3 𝒒1 𝑛4 𝑛1 𝑚4 𝑚1 𝑛3 𝑛2 𝑚3 𝑚2 𝒒2 Cohesive layer 𝒙t 𝒒1 𝒒3 𝒒2 𝒙b Figure 5.1. Illustration of cohesive elements 19, 20 and ±29 As a comparison to other elements, the cohesive “strain” is the separation distance (length) between the two surfaces, and the cohesive stress (force per area) is its Cohesive Elements LS-DYNA Theory Manual conjugate with respect to the energy surface density (energy per area). Cohesive elements 21 and 22 are pentahedral versions of elements 19 and 20, respectively, where the top and bottom surface are triangles. These elements are not treated here per se, but the only difference is that the iso-parametric interpolation functions change. 5.1 Kinematics For this presentation we refer to Figure 5.1 for an illustration. Let be the separation of the cohesive layer in the local system, where 𝒅 = 𝑸𝑻 (𝒙𝑡 − 𝒙𝑏) − 𝒅0, 𝑸 = [𝒒1 𝒒2 𝒒3], (5.1) (5.2) is the local coordinate system and 𝒙𝑡 and 𝒙𝑏 are global coordinates on the top and bottom surfaces for a given iso-parametric coordinate (𝜉 , 𝜂). The distance vector 𝒅0 represents the initial gap for cases where the cohesive interface has a nonzero thickness, so 𝒅 = 𝟎 initially. For cohesive element 19 the separation is given directly from the solid element geometries (sum over i) where and 𝒙𝑡 = 𝒙𝑖 𝑛𝑁𝑖(𝜉 , 𝜂), 𝒙𝑏 = 𝒙𝑖 𝑚𝑁𝑖(𝜉 , 𝜂), 𝑁𝑖(𝜉 , 𝜂) = (1 + 𝜉 𝑖𝜉 )(1 + 𝜂𝑖𝜂), 𝜉 ∗ = [−1, 1, 1, −1], 𝜂∗ = [−1, −1, 1, 1], (5.3) (5.4) (5.5) are the in-plane shape functions. From here and onwards, superscripts n and m denote 𝑚 are the nodal coordinates the top and bottom surfaces, respectively, and thus 𝒙𝑖 associated with the two surfaces. For cohesive elements 20 and ±29, the separation 𝒅 is updated using an incremental formulation and we have 𝑛 and 𝒙𝑖 𝒅 ̇= 𝑸𝑇(𝒙̇𝑡 − 𝒙̇𝑏) + 𝑸̇𝑇𝑸𝒅. (5.6) Furthermore, for cohesive element 20 we have (sum over i) LS-DYNA Theory Manual Cohesive Elements 𝒙̇𝑡 = {𝒙̇𝑖 𝑛 − 𝒙̇𝑏 = {𝒙̇𝑖 𝑚 + 𝝎𝑖 𝑛 × 𝒏𝑡} 𝑁𝑖(𝜉 , 𝜂), 𝝎𝑖 𝑚 × 𝒏𝑏} 𝑁𝑖(𝜉 , 𝜂), (5.7) where the thicknesses of the two shells adjacent to the cohesive layer are denoted t, currently assumed to be the same for the both. In these equations, 𝒏𝑡 and 𝒏𝑏 are the top and bottom shell normal, initially equal to 𝒒3 but they may evolve independently with time. For cohesive element ±29 we instead have 𝒙̇𝑡 = {𝒙̇1 𝑛 + 𝜉 𝑛 × 𝒏𝑡} 𝐱̇𝑏 = {𝐱̇4 𝑚 + 𝜉 𝑚 × 𝐧𝑏} 𝝎1 𝑚 and 𝝎𝑖 𝝎4 1 − 𝜂 1 − 𝜂 + {𝒙̇2 𝑛 + 𝜉 + {𝐱̇3 𝑚 + 𝜉 𝝎2 𝑛 × 𝒏𝑡} 𝝎3 𝑚 × 𝐧𝑏} , 1 + 𝜂 1 + 𝜂 (5.8) . 𝑛 denote nodal rotational velocities, and also note that In these expressions 𝝎𝑖 for evaluation the velocities of 𝒙𝑡 and 𝒙𝑏 we assume that the fiber pointing from assumed mid layer coincides with that of the coordinate axes. This is in analogy to how the Belytschko-Tsay element is treating the fiber vectors and presumably enhances robustness of the elements. Note also that the shell normal are in this case initially equal to 𝒒1. For the local coordinate system, cohesive elements 19 and 20 evaluate this according to the invariant node numbering approach for shells using the mid layer node coordinates 𝒙̅𝑖 = 𝑛 + 𝒙𝑖 𝒙𝑖 , 𝑖 = 1,2,3,4, 𝒆1 = 𝒆2 = 𝒙̅3 − 𝒙̅1 ∣𝒙̅3 − 𝒙̅1∣ 𝒙̅4 − 𝒙̅2 |𝒙̅4 − 𝒙̅2| , , 𝒒1 = − 𝒒2 = , 𝒆1 + 𝒆2 |𝒆1 + 𝒆2| 𝒆1 − 𝒆2 |𝒆1 − 𝒆2| , as follows. First let and then followed by 𝒒3 = 𝒒1 × 𝒒2. Cohesive element +29 starts by computing 𝑛 + 𝒙3 𝒙2 𝑛 + 𝒙3 ∣𝒙2 𝒒2 = 𝑚 − 𝒙1 𝑚 − 𝒙1 𝑛 − 𝒙4 𝑚∣ 𝑛 − 𝒙4 , (5.9) (5.10) (5.11) (5.12) (5.13) Cohesive Elements LS-DYNA Theory Manual followed by and 𝒒 = 𝒙4 𝑛 + 𝒙3 𝑛 − 𝒙1 𝑚, 𝑚 − 𝒙2 𝒒3 = 𝒒 − 𝒒2𝒒𝑇𝒒2 |𝒒 − 𝒒2𝒒𝑇𝒒2| , 𝒒1 = 𝒒2 × 𝒒3. Cohesive element -29 starts by computing 𝑛 + 𝒙3 𝒙2 𝑛 + 𝒙3 ∣𝒙2 𝒒2 = 𝑚 − 𝒙1 𝑚 − 𝒙1 𝑛 − 𝒙4 𝑚∣ 𝑛 − 𝒙4 , followed by 𝒒 = ( and (𝒙3 ∣(𝒙3 𝑛 − 𝒙1 𝑛 − 𝒙1 𝑛) × (𝒙4 𝑛) × (𝒙4 𝑛) 𝑛 − 𝒙2 𝑛)∣ 𝑛 − 𝒙2 + (𝒙3 ∣(𝒙3 𝑚 − 𝒙1 𝑚 − 𝒙1 𝑚) × (𝒙4 𝑚) × (𝒙4 𝑚 − 𝒙2 𝑚 − 𝒙2 𝑚) 𝑚)∣ 𝒒1 = 𝒒 − 𝒒2𝒒𝑇𝒒2 |𝒒 − 𝒒2𝒒𝑇𝒒2| , 𝒒3 = 𝒒1 × 𝒒2. (5.14) (5.15) (5.16) (5.17) ), (5.18) (5.19) (5.20) Thus, in pure out-of-plane shear, type +29 will initially have pure tangential traction in the 𝑞1-direction, that turns into a normal traction in the 𝑞3-direction, as the separation increases. Element type -29, however, will only have tangential traction in this case. 5.2 Constitutive law The cohesive constitutive law amounts to determine the normal and shear stress, expressed here as the stress vector 𝝈, as function of the separation vector 𝒅, 𝝈 = 𝝈(𝒅, … ). The typical appearance of each component of this vector is illustrated in Figure 5.2., the interface behaves elastically up to a critical separation distance 𝑑𝑒 and peak stress 𝜎𝑒 after which damage commences. The interface is damaged and failure occur at a certain critical separation distance 𝑑𝑐, the unloading is typically elastic as indicated by the dashed arrow. For detailed information on individual cohesive constitutive laws we refer to the materials section. LS-DYNA Theory Manual Cohesive Elements 𝜎 𝜎𝑒 𝑑𝑒 𝑑𝑐 𝑑 Figure 5.2.Common stress versus separation for a cohesive interface 5.3 Nodal forces The principle of virtual work states that (sum over i) = {𝒙̇𝑖 𝑛}𝑇𝒇𝑖 𝑚}𝑇𝒇𝑖 𝑚}𝑇𝒓𝑖 𝑚 + {𝒙̇𝑖 𝑛 + {𝝎𝑖 𝑚 + {𝝎𝑖 𝑗 and 𝒓𝑖 ∫ 𝒅 ̇𝑇𝝈𝑑𝐴 𝑗 is the nodal force and moment for node i on element j, respectively. The where 𝒇𝑖 area A represents the cohesive mid layer spanned by the iso-parametric representation and this is used to identify the nodal forces and moments. In the following we work out the details for cohesive element ±29. Cohesive elements 19 and 20 are treated analogous. Using Equation (5.6) we also have 𝑛}𝑇𝒓𝑖 𝑛, (5.21) ∫ 𝐝̇𝑇𝛔𝑑𝐴 𝑇𝐐𝛔𝑑𝐴 = ∫ 𝐱̇𝑡 𝑇𝐐𝛔𝑑𝐴 − ∫ 𝐱̇𝑏 − ∫ 𝐝𝑇𝐐̇ 𝑇𝐐𝛔𝑑𝐴 , (5.22) and before continuing we rewrite (5.8) as − {𝝎1 𝑛}𝑇𝑹𝑡 𝑇 = {𝒙̇1 𝒙̇𝑡 where 𝑹∗ is the linear operator defined by 𝑛}𝑇 1 − 𝜂 𝑚}𝑇 1 − 𝜂 𝑇 1 − 𝜂 𝑇 1 − 𝜂 𝑇 = {𝒙̇4 𝒙̇𝑏 𝑚}𝑇𝑹𝑏 − {𝝎4 + {𝒙̇2 + {𝒙̇3 𝑛}𝑇 1 + 𝜂 𝑚}𝑇 1 + 𝜂 − {𝝎2 𝑛}𝑇𝑹𝑡 − {𝝎3 𝑚}𝑇𝑹𝑏 𝑇 1 + 𝜂 𝑇 1 + 𝜂 , and insert this into the right of (5.22) which after some simplifications gives 𝑹∗𝝎 = 𝒏∗ × 𝝎 (5.23) , (5.24) Cohesive Elements LS-DYNA Theory Manual ∫ 𝒅 ̇𝑇𝝈𝑑𝐴 = − ∫ 𝒅𝑇𝑸̇𝑇𝑸𝝈𝑑𝐴 +{𝐱̇1 𝑛}𝑇 ∫ ( 1 − 𝜂 ) 𝐐𝛔𝑑𝐴 + {𝝎1 𝑛}𝑇 ∫ (− 1 − 𝜂 ) 𝐑𝑡 𝑇𝐐𝛔𝑑𝐴 +{𝒙̇2 𝑛}𝑇 ∫ ( 1 + 𝜂 ) 𝑸𝝈𝑑𝐴 + {𝝎2 𝑛}𝑇 ∫ (− 1 + 𝜂 ) 𝑹𝑡 𝑇𝑸𝝈𝑑𝐴 (5.25) +{𝒙̇4 𝑚}𝑇 ∫ (− 1 − 𝜂 ) 𝑸𝝈𝑑𝐴 + {𝝎4 𝑚}𝑇 ∫ ( 1 − 𝜂 ) 𝑹𝑏 𝑇𝑸𝝈𝑑𝐴 +{𝒙̇3 𝑚}𝑇 ∫ (− 1 + 𝜂 ) 𝑸𝝈𝑑𝐴 + {𝝎3 𝑚}𝑇 ∫ ( 1 + 𝜂 ) 𝑹𝑏 𝑇𝑸𝝈𝑑𝐴 . If the first term on the right hand side of (5.25) is neglected we can, using (5.21) and (5.25), identify the nonzero nodal forces and moments 𝑛 = ∫ ( 𝒇1 1 − 𝜂 𝑛 = ∫ ( 𝒇2 1 + 𝜂 ) 𝑸𝝈𝑑𝐴, 𝑛 = − 𝒓1 ) 𝑸𝝈𝑑𝐴, 𝑛 = − 𝒓2 1 − 𝜂 ∫ ( 1 + 𝜂 ∫ ( 𝜉 ) 𝑹𝑡 𝑇𝑸𝝈𝑑𝐴, 𝜉 ) 𝑹𝑡 𝑇𝑸𝝈𝑑𝐴, (5.26) 𝑚 = −𝒇2 𝒇3 𝑛, 𝒓3 𝑚 = 𝑚 = −𝒇1 𝒇4 𝑛, 𝒓4 𝑚 = 1 + 𝜂 ∫ ( 1 − 𝜂 ∫ ( 𝜉 ) 𝑹𝑏 𝑇𝑸𝝈𝑑𝐴, 𝜉 ) 𝑹𝑏 𝑇𝑸𝝈𝑑𝐴. In the implementation these integrals are evaluated using 4-point Gaussian quadrature, where the integration point locations are given by 𝜉∗ = ⎢⎡− ⎣ √3 , √3 , √3 , − ⎥⎤, √3⎦ 𝜂∗ = ⎢⎡− ⎣ √3 , − √3 , √3 , ⎥⎤. √3⎦ Thus an integral is evaluated as ∫ 𝜙(𝜉 , 𝜂)𝛔𝑑𝐴 ≈ ∑ 𝜙(𝜉𝑖, 𝜂𝑖)𝛔𝑖𝐴𝑖 , 𝑖=1 (5.27) (5.28) LS-DYNA Theory Manual Cohesive Elements where 𝜙 is an arbitrary function of the iso-parametric coordinates, 𝐴𝑖 in the right hand side stands for the area of the cohesive layer and 𝛔𝑖 is the cohesive interface stress, both evaluated at and with respect to integration point i. 5.4 Drilling constraint in shell ±29 From (5.8) and the picture of shell type ±29 in Figure 5.1, we see that rotational velocities with respect to the adjacent shell normals will not induce translational velocities in the integration points, so a stabilization scheme is applied. To this end we 𝑚, 𝑖 = 1,2, 𝑗 = 3,4, distances that are introduce the generalized drilling strains δ𝑖 incremented by their respective velocities 𝑛 and δ𝑗 𝑛 = 𝒏𝑡 𝛿 ̇ 𝑚 = 𝒏𝑏 𝛿 ̇ 𝑇{𝝎𝑖 𝑇{𝝎𝑗 𝑛𝑑21 − 𝑹21(𝒙̇2 𝑚𝑑34 − 𝑹34(𝒙̇3 𝑛 − 𝒙̇1 𝑚 − 𝒙̇4 𝑛)}, 𝑖 = 1,2, 𝑚)}, 𝑗 = 3,4, where 𝑑21 = ∣𝒙2 𝑑34 = ∣𝒙3 𝑛∣, 𝑛 − 𝒙1 𝑚∣, 𝑚 − 𝒙4 and we make use of the following definitions for arbitrary vector 𝐯, 𝑹21𝒗 = 𝑹34𝒗 = 𝑑21 𝑑34 (𝒙2 𝑛 − 𝒙1 𝑛) × 𝒗, (𝒙3 𝑚 − 𝒙4 𝑚) × 𝒗. (5.29) (5.30) (5.31) A characteristic material stiffness 𝐸, typically a fraction of the elastic stiffness of the underlying cohesive material, is used to set up the drilling stress 𝑛, 𝑛 = 𝐸𝛿𝑖 𝜍𝑖 𝑚, 𝑚 = 𝐸𝛿𝑗 𝜍𝑗 𝑖 = 1,2, 𝑗 = 3,4, (5.32) and the stabilization nodal forces are evaluated as Cohesive Elements LS-DYNA Theory Manual 𝑇 𝐧𝑡, 𝐫1 𝑛 = 𝐴𝜍2 𝑚 = 𝐴𝜍3 𝑇 𝐧𝑏, 𝐫4 and these forces and moments are added to the structural ones in the previous section. 𝑛+𝜍2 𝑛 = 𝐴(𝜍1 𝐟1 𝑛 = −𝐟1 𝐟2 𝑚 = −𝐟4 𝐟3 𝑚+𝜍4 𝑛 = 𝐴𝜍1 𝑛𝑑21𝐧𝑡, 𝑚𝑑34𝐧𝑏, 𝑚 = 𝐴𝜍4 𝑛)𝐑21 𝑛, 𝐫2 𝑚, 𝐫3 𝑚)𝐑34 𝑚 = 𝐴(𝜍3 𝐟4 𝑚𝑑34𝐧𝑏, 𝑛𝑑21𝐧𝑡, (5.33) 5.5 Rotational masses in shell ±29 The rotational mass in shell ±29 is determined from a simple energy criterion. Assuming that the cohesive layer is thin and the layer spins with a rotational velocity 𝜔 around axis 𝒒2, the kinetic energy from the nodal rotational masses 𝑚𝑟 is 𝑊 = (𝑚𝑟 + 𝑚𝑟 + 𝑚𝑟 + 𝑚𝑟)𝜔2 = 2𝑚𝑟𝜔2. (5.34) This is compared to the corresponding kinetic energy for an equivalent solid type 19 cohesive layer, using that the shell type ±29 translational nodal mass 𝑚𝑡 is twice that of the solid type 19 nodal masses, 𝑊 = 𝑚𝑡 ( + 𝑚𝑡 + 𝑚𝑡 + 𝑚𝑡 + 𝑚𝑡 + 𝑚𝑡 + 𝑚𝑡 + 𝑚𝑡 ) ( 𝜔) = 𝑚𝑡𝑡2𝜔2, which results in 𝑚𝑟 = 𝑚𝑡𝑡2. (5.35) (5.36) 5.6 Stiffness matrix in shell ±29 The stiffness matrix is the sum of contributions from the constitutive law and the drilling force, and is for simplicity implemented for a force free configuration, i.e., 𝝈 = 𝟎, 𝝇 = 𝟎, (5.37) where we have used the notation LS-DYNA Theory Manual Cohesive Elements 𝝇 = 𝜍1 ⎤ ⎡ 𝜍2 ⎥ ⎢ . ⎥ ⎢ 𝜍3 ⎥ ⎢ 𝑚⎦ 𝜍4 ⎣ (5.38) For a given integration point and referring to Equation (5.26) and (5.33), we collect these nodal force triplets into complete nodal vectors 𝒇 and 𝒈, associated with the constitutive and drilling part, respectively. That is, 𝒇 = 𝒇1 ⎤ ⎡ 𝒓1 ⎥ ⎢ ⎥ ⎢ 𝒇2 ⎥ ⎢ ⎥ ⎢ 𝒓2 ⎥ ⎢ , ⎥ ⎢ 𝒇3 ⎥ ⎢ ⎥ ⎢ 𝒓3 ⎥ ⎢ 𝒇4 ⎥ ⎢ 𝑚⎦ 𝒓4 ⎣ (5.39) and the same expression holds for 𝒈. Likewise we let 𝒗 be the collection of nodal velocities, i.e., 𝒗 = 𝒙̇1 ⎤ ⎡ 𝝎1 ⎥ ⎢ ⎥ ⎢ 𝒙̇2 ⎥ ⎢ 𝝎2 ⎥ ⎢ ⎥ ⎢ 𝒙̇3 ⎥ ⎢ ⎥ ⎢ 𝝎3 ⎥ ⎢ 𝒙̇4 ⎥ ⎢ 𝑚⎦ 𝝎4 ⎣ , (5.40) and note that we can identify generalized strain-displacement matrices 𝑩𝑓 (3 by 24 matrix) and 𝑩𝑔 (4 by 24 matrix) from (5.6) and (5.8) as well as (5.29) so that 𝒅 ̇= 𝑩𝑓 𝒗, 𝜹 ̇ = 𝑩𝑔𝒗, where we have collected the drilling kinematic velocities in a vector 𝜹 ̇ = 𝛿 ̇ ⎤ ⎡ 𝛿 ̇ ⎥ ⎢ ⎥ ⎢ ⎥ ⎢ 𝛿 ̇ ⎥ ⎢ 𝑚⎦ 𝛿 ̇ ⎣ With this notation we can rewrite (5.26) and (5.33) into a more compact form (5.41) (5.42) Cohesive Elements LS-DYNA Theory Manual 𝒇 = 𝑩𝑓 𝑇𝝈𝐴, 𝒈 = 𝑩𝑔 𝑇𝝇𝐴, (5.43) with 𝐴 here being the area of the integration point of interest. The stiffness matrix is then simply the differentiation of these force vectors with respect to the nodal coordinates, and by using (5.32), (5.37) and the chain rule of differentiation we get 𝑲𝑓 = 𝑩𝑓 𝑩𝑓 𝐴, 𝑇 𝜕𝝈 𝜕𝒅 𝑇𝑩𝑔𝐴, 𝑲𝑔 = 𝐸𝑩𝑔 (5.44) where 𝜕𝝈/𝜕𝒅 is the constitutive tangent from the cohesive material used. LS-DYNA Theory Manual Belytschko Beam 6 Belytschko Beam The Belytschko beam element formulation [Belytschko et al. 1977] is part of a family of structural finite elements, by Belytschko and other researchers that employ a ‘co-rotational technique’ in the element formulation for treating large rotation. This section discusses the co-rotational formulation, since the formulation is most easily described for a beam element, and then describes the beam theory used to formulate the co-rotational beam element. 6.1 Co-rotational Technique from In any large displacement formulation, the goal is to separate the deformation displacements the deformation displacements give rise to strains and the associated generation of strain energy. This separation is usually accomplished by comparing the current configuration with a reference configuration. the rigid body displacements, as only The current configuration is a complete description of the deformed body in its current spatial location and orientation, giving locations of all points (nodes) comprising the body. The reference configuration can be either the initial configuration of the body, i.e., nodal locations at time zero, or the configuration of the body at some other state (time). Often the reference configuration is chosen to be the previous configuration, say at time 𝑡𝑛 = 𝑡𝑛+1 − Δ𝑡. The choice of the reference configuration determines the type of deformations that will be computed: total deformations result from comparing the current configuration with the initial configuration, while incremental deformations result from comparing with the previous configuration. In most time stepping (numerical) Lagrangian formulations, incremental deformations are used because they result in significant simplifications of other algorithms, chiefly constitutive models. Belytschko Beam LS-DYNA Theory Manual b2 ¯Y b1 ^ e0 e0 X¯ (a) Initial Configuration ^ Figure 6.1. Co-rotational coordinate system: (a) initial configuration, (b) rigid rotational configuration and (c) deformed configuration. A direct comparison of the current configuration with the reference configuration does not result in a determination of the deformation, but rather provides the total (or incremental) displacements. We will use the unqualified term displacements to mean either the total displacements or the incremental displacements, depending on the choice of the reference configuration as the initial or the last state. This is perhaps most obvious if the reference configuration is the initial configuration. The direct comparison of the current configuration with the reference configuration yields displacements, which contain components due to deformations and rigid body motions. The task remains of separating the deformation and rigid body displacements. The deformations are usually found by subtracting from the displacements an estimate of the rigid body displacements. Exact rigid body displacements are usually only known for trivial cases where they are prescribed a priori as part of a displacement field. The co-rotational formulations provide one such estimate of the rigid body displacements. The co-rotational formulation uses two types of coordinate systems: one system associated with each element, i.e., element coordinates which deform with the element, and another associated with each node, i.e., body coordinates embedded in the nodes. (The term ‘body’ is used to avoid possible confusion from referring to these coordinates as ‘nodal’ coordinates. Also, in the more general formulation presented in [Belytschko et al., 1977], the nodes could optionally be attached to rigid bodies. Thus the term ‘body coordinates’ refers to a system of coordinates in a rigid body, of which a node is a special case.) These two coordinate systems are shown in the upper portion of Figure 6.1. The element coordinate system is defined to have the local x-axis 𝐱̂ originating at node 𝐼 and terminating at node 𝐽; the local y-axis 𝐲̂ and, in three dimension, the local z- axis 𝐳̂, are constructed normal to 𝐱̂. The element coordinate system (𝐱̂, 𝐲̂, 𝐳̂) and associated unit vector triad (𝐞1, 𝐞2, 𝐞3) are updated at every time step by the same technique used to construct the initial system; thus the unit vector e1 deforms with the element since it always points from node 𝐼 to node 𝐽. LS-DYNA Theory Manual Belytschko Beam ^ ^ e2 ¯Y b2 e1 b1 X¯ (b) Rigid Rotation Configuration Figure 6.2. Co-rotational coordinate system: (a) initial configuration, (b) rigid rotational configuration and (c) deformed configuration. The embedded body coordinate system is initially oriented along the principal inertial axes; either the assembled nodal mass or associated rigid body inertial tensor is used in determining the inertial principal values and directions. Although the initial orientation of the body axes is arbitrary, the selection of a principal inertia coordinate system simplifies the rotational equations of motion, i.e., no inertial cross product terms are present in the rotational equations of motion. Because the body coordinates are fixed in the node, or rigid body, they rotate and translate with the node and are updated by integrating the rotational equations of motion, as will be described subsequently. The unit vectors of the two coordinate systems define rotational transformations between the global coordinate system and each respective coordinate system. These transformations operate on vectors with global components 𝐀 = (𝐴𝑥, 𝐴𝑦, 𝐴𝑧), body coordinates components 𝐀̅̅̅̅̅̅ = (𝐴̅𝑥, 𝐴̅𝑦, 𝐴̅𝑧), and element coordinate components  = (𝐴̂𝑥, 𝐴̂𝑦, 𝐴̂𝑧) which are defined as: 𝐀 = {⎧𝐴𝑥 }⎫ 𝐴𝑦 𝐴𝑧⎭}⎬ ⎩{⎨ = 𝑏1𝑥 ⎡ 𝑏1𝑦 ⎢⎢ 𝑏1𝑧 ⎣ 𝑏2𝑥 𝑏2𝑦 𝑏2𝑧 𝑏3𝑥 ⎤ 𝑏3𝑦 ⎥⎥ 𝑏3𝑧⎦ {{⎧𝐴̅𝑥 }}⎫ 𝐴̅𝑦 }}⎬ {{⎨ 𝐴̅𝑧⎭ ⎩ = [𝛌]{𝐀̅̅̅̅̅̅}, (6.1) where 𝑏𝑖𝑥, 𝑏𝑖𝑦, 𝑏𝑖𝑧 are the global components of the body coordinate unit vectors. Similarly for the element coordinate system: 𝐀 = {⎧𝐴𝑥 }⎫ 𝐴𝑦 𝐴𝑧⎭}⎬ ⎩{⎨ = 𝑒1𝑥 ⎢⎡ 𝑒1𝑦 𝑒1𝑧 ⎣ 𝑒2𝑥 𝑒2𝑦 𝑒2𝑧 𝑒3𝑥 ⎥⎤ 𝑒3𝑦 𝑒3𝑧⎦ ⎧𝐴̂𝑥 ⎫ }} {{ 𝐴̂𝑦 ⎬ ⎨ }} {{ 𝐴̂𝑧⎭ ⎩ = [𝛍]{𝐀̂}, (6.2) where 𝑒𝑖𝑥, 𝑒𝑖𝑦, 𝑒𝑖𝑧 are the global components of the element coordinate unit vectors. The inverse transformations are defined by the matrix transpose, i.e., {𝐀̅̅̅̅̅̅} = [𝛌]T{𝐀} {𝐀̂} = [𝛍]T{𝐀}, (6.3) Belytschko Beam LS-DYNA Theory Manual ¯Y b2 ^ e2 e1 b1 e0 X¯ (c) Deformed Configuration ^ Figure 6.3. Co-rotational coordinate system: (a) initial configuration, (b) rigid rotational configuration and (c) deformed configuration. since these are proper rotational transformations. The following two examples illustrate how the element and body coordinate system are used to separate the deformations and rigid body displacements from the displacements: Rigid Rotation. First, consider a rigid body rotation of the beam element about node 𝐼, as shown in the center of Figure 6.2, i.e., consider node 𝐼 to be a pinned connection. Because the beam does not deform during the rigid rotation, the orientation of the unit vector 𝐞1 in the initial and rotated configuration will be the same with respect to the body coordinates. If the body coordinate components of the initial element unit vector 0 were stored, they would be identical to the body coordinate components of the 𝐞1 current element unit vector e1. Deformation Rotation. Next, consider node 𝐼 to be constrained against rotation, i.e., a clamped connection. Now node 𝐽 is moved, as shown in the lower portion of Figure 6.3, causing the beam element to deform. The updated element unit vector e1 is constructed and its body coordinate components are compared to the body coordinate components 0. Because the body coordinate system did not of the original element unit vector 𝐞1 rotate, as node I was constrained, the original element unit vector and the current element unit vector are not colinear. Indeed, the angle between these two unit vectors is the amount of rotational deformation at node I, i.e., 𝐞1 × 𝐞1 0 = 𝜃ℓ𝐞3. (6.4) Thus the co-rotational formulation separates the deformation and rigid body deformations by using: • a coordinate system that deforms with the element, i.e., the element coordinates; • or a coordinate system that rigidly rotates with the nodes, i.e., the body coordinates; LS-DYNA Theory Manual Belytschko Beam Then it compares the current orientation of the element coordinate system with the initial element coordinate system, using the rigidly rotated body coordinate system, to determine the deformations. 6.2 Belytschko Beam Element Formulation The deformation displacements used in the Belytschko beam element formulation are: where, 𝐝̂T = {𝛿𝐼𝐽, 𝜃̂ 𝑥𝐽𝐼, 𝜃̂ 𝑦𝐼, 𝜃̂ 𝑦𝐽, 𝜃̂ 𝑧𝐼, 𝜃̂ 𝑧𝐽}, (6.5) 𝛿𝐼𝐽 = length change 𝜃̂ 𝑥𝐽𝐼 = torsional deformation 𝑧𝐼, 𝜃̂ 𝑧𝐽 = bending rotation deformations 𝑦𝐼, 𝜃̂ 𝜃̂ 𝑦𝐽, 𝜃̂ The superscript ^ emphasizes that these quantities are defined in the local element coordinate system, and 𝐼 and 𝐽 are the nodes at the ends of the beam. The beam deformations, defined above in Equation (6.5), are the usual small displacement beam deformations (see, for example, [Przemieniecki 1986]). Indeed, one advantage of the co-rotational formulation is the ease with which existing small displacement element formulations can be adapted to a large displacement formulation having small deformations in the element system. Small deformation theories can be easily accommodated because the definition of the local element coordinate system is independent of rigid body rotations and hence deformation displacement can be defined directly. 6.2.1 Calculation of Deformations The elongation of the beam is calculated directly from the original nodal coordinates (𝑋𝐼, 𝑌𝐼, 𝑍𝐼) and the total displacements (𝑢𝑥𝐼, 𝑢𝑦𝐼, 𝑢𝑧𝐼): 𝛿𝐼𝐽 = where 𝑙 + 𝑙𝑜 [2(𝑋𝐽𝐼𝑢𝑥𝐽𝐼 + 𝑌𝐽𝐼𝑢𝑦𝐽𝐼 + 𝑍𝐽𝐼𝑢𝑧𝐽𝐼) + 𝑢𝑥𝐽𝐼 2 + 𝑢𝑦𝐽𝐼 2 + 𝑢𝑧𝐽𝐼 2 ], 𝑋𝐽𝐼 = 𝑋𝐽 − 𝑋𝐼 𝑢𝑥𝐽𝐼 = 𝑢𝑥𝐽 − 𝑢𝑥𝐼, etc. (6.6) (6.7) The deformation rotations are calculated using the body coordinate components 0, as outlined in of the original element coordinate unit vector along the beam axis, i.e., 𝐞1 0 the previous section. Because the body coordinate components of initial unit vector 𝐞1 rotate with the node, in the deformed configuration it indicates the direction of the Belytschko Beam LS-DYNA Theory Manual 0 beam’s axis if no deformations had occurred. Thus comparing the initial unit vector 𝐞1 with its current orientation 𝐞1 indicates the magnitude of deformation rotations. Forming the vector cross product between 𝐞1 0 and 𝐞1: 𝐞1 × 𝐞1 0 = 𝜃̂ 𝑦𝐞2 + 𝜃̂ 𝑧𝐞3, (6.8) where 𝜃̂ 𝑦 = is the incremental deformation about the local 𝑦̂ axis 𝜃̂ 𝑧 = is the incremental deformation about the local 𝑧̂ axis The calculation is most conveniently performed by transforming the body components of the initial element vector into the current element coordinate system: ⎫ ⎧𝑒 ̂1𝑥 }} {{ 0 𝑒 ̂1𝑦 ⎬ ⎨ }} {{ 0 ⎭ 𝑒 ̂1𝑧 ⎩ = [𝛍]T[𝛌] ⎫ ⎧𝑒 ̅1𝑥 }} {{ 0 𝑒 ̅1𝑦 ⎬ ⎨ }} {{ 0 ⎭ 𝑒 ̅1𝑧 ⎩ . Substituting the above into Equation (4.10) 𝐞1 × 𝐞1 0 = det 𝐞1 0 𝑒 ̂1𝑥 ⎡ ⎢ ⎣ 𝐞2 0 𝑒 ̂1𝑦 𝐞3 0 𝑒 ̂1𝑧 Thus, ⎤ = −𝑒 ̂1𝑧 ⎥ ⎦ 0 𝐞2 + 𝑒 ̂1𝑦 0 𝐞3 = 𝜃̂ 𝑦𝐞2 + 𝜃̂ 𝑧𝐞3. 𝜃̂ 𝑦 = −𝑒 ̂1𝑧 0 . 𝜃̂ 𝑧 = 𝑒 ̂1𝑦 (6.9) (6.10) (6.11) The torsional deformation rotation is calculated from the vector cross product of initial unit vectors, from each node of the beam, that were normal to the axis of the 0 could also be used. The result from this 0 and 𝑒 ̂3𝐽 beam, i.e., 𝑒 ̂2𝐼 vector cross product is then projected onto the current axis of the beam, i.e., 0 ; note that 𝑒 ̂3𝐼 0 and 𝑒 ̂2𝐽 𝜃̂ 𝑥𝐽𝐼 = 𝐞1 ⋅ (𝐞̂2𝐼 0 × 𝐞̂2𝐽 0 ) = 𝐞1 ⋅ det 𝐞2 0 𝑒 ̂𝑦2𝐼 0 𝑒 ̂𝑦2𝐽 𝐞1 ⎡ 0 𝑒 ̂𝑥2𝐼 ⎢⎢ 0 𝑒 ̂𝑥2𝐽 ⎣ 0 and 𝑒 ̅2𝐽 𝐞3 0 𝑒 ̂𝑧2𝐼 0 𝑒 ̂𝑧2𝐽 ⎤ ⎥⎥ ⎦ = 𝑒 ̂𝑦2𝐼 0 𝑒 ̂𝑧2𝐽 0 − 𝑒 ̂𝑦2𝐽 0 . 0 𝑒 ̂𝑧2𝐼 (6.12) Note that the body components of 𝑒 ̅2𝐼 coordinate system before performing the indicated vector products. 0 are transformed into the current element 6.2.2 Calculation of Internal Forces There are two methods for computing the internal forces for the Belytschko beam element formulation: 1. 2. functional forms relating the overall response of the beam, e.g., moment- curvature relations, direct through-the-thickness integration of the stress. {⎧𝜃̂ }⎫ 𝑦𝐼 𝑦𝐽⎭}⎬ ⎩{⎨ 𝜃̂ 𝜃̂ 𝑧𝐼 𝜃̂ 𝑧𝐽 LS-DYNA Theory Manual Belytschko Beam Currently only the former method, as explained subsequently, is implemented; the direct integration method is detailed in [Belytschko et al., 1977]. Axial Force. The internal axial force is calculated from the elongation of the beam 𝛿, as given by Equation (6.6), and an axial stiffness: 𝑓 ̂ 𝑥𝐽 = 𝐾𝑎𝛿, (6.13) where 𝐾𝑎 = 𝐴𝐸 𝑙0 = is the axial stiffness 𝐴 = cross sectional area of the beam 𝐸 = Young's Modulus 𝑙0 = original length of the beam Bending Moments. The bending moments are related to the deformation rotations by { 𝑚̂𝑦𝐼 𝑚̂𝑦𝐽 } = 𝐾𝑦 1 + 𝜙𝑦 4 + 𝜙𝑦2 − 𝜙𝑦 [ 2 − 𝜙𝑦4 + 𝜙𝑦 ] , (6.14a) 4 + 𝜙𝑧2 − 𝜙𝑧 2 − 𝜙𝑧4 + 𝜙𝑧 where Equation (6.14a) is for bending in the 𝐱̂ − 𝐳̂ plane and Equation (6.14b) is for bending in the 𝐱̂ − 𝐲̂ plane. The bending constants are given by 𝑚̂𝑧𝐼 { 𝑚̂𝑧𝐽 (6.14b) } = ] { }, [ 𝐾𝑧 1 + 𝜙𝑧 𝑏 = 𝐾𝑦 𝑏 = 𝐾𝑧 𝐸𝐼𝑦𝑦 𝑙0 𝐸𝐼𝑧𝑧 𝑙0 𝐼𝑦𝑦 = ∫ ∫ 𝑧̂2𝑑𝑦̂𝑑𝑧̂ 𝐼𝑧𝑧 = ∫ ∫ 𝑦̂2𝑑𝑦̂𝑑𝑧̂ 𝜙𝑦 = 𝜙𝑧 = 12𝐸𝐼𝑦𝑦 𝐺𝐴𝑠𝑙2 12𝐸𝐼𝑧𝑧 𝐺𝐴𝑠𝑙2 . (6.15a) (6.15b) (6.15c) (6.15d) (6.15e) (6.15f) Hence 𝜙 is the shear factor, 𝐺 the shear modulus, and 𝐴𝑠 is the effective area in shear. Torsional Moment. The torsional moment is calculated from the torsional deformation rotation as Belytschko Beam LS-DYNA Theory Manual where and, 𝑚̂𝑥𝐽 = 𝐾𝑡𝜃̂ 𝑥𝐽𝐼, 𝐾𝑡 = 𝐺𝐽 𝑙0 , 𝐽 = ∫ ∫ 𝑦̂𝑧̂𝑑𝑦̂𝑑𝑧̂. (6.16) (6.17) (6.18) The above forces are conjugate to the deformation displacements given previously in Equation (6.5), i.e., 𝐝̂T = {𝛿𝐼𝐽, 𝜃̂ 𝑥𝐽𝐼, 𝜃̂ 𝑦𝐼, 𝜃̂ 𝑦𝐽, 𝜃̂ 𝑧𝐼, 𝜃̂ 𝑧𝐽}, where And with 𝐝̂T𝐟 ̂ = 𝑊int. 𝐟 ̂ T = {𝑓 ̂ 𝑥𝐽, 𝑚̂𝑥𝐽, 𝑚̂𝑦𝐼, 𝑚̂𝑦𝐽, 𝑚̂𝑧𝐼, 𝑚̂𝑧𝐽}. The remaining internal force components are found from equilibrium: 𝑓 ̂ 𝑧𝐼 = − 𝑥𝐼 = −𝑓 ̂ 𝑓 ̂ 𝑥𝐽 𝑚̂𝑦𝐼 + 𝑚̂𝑦𝐽 𝑙0 𝑚̂𝑧𝐼 + 𝑚̂𝑧𝐽 𝑙0 𝑓 ̂ 𝑦𝐽 = − 𝑚̂𝑥𝐼 = −𝑚̂𝑥𝐽 𝑧𝐼 = −𝑓 ̂ 𝑓 ̂ 𝑧𝐽 𝑦𝐼 = −𝑓 ̂ 𝑓 ̂ 𝑦𝐽 (6.19) (6.20) (6.21) (6.22) 6.2.3 Updating the Body Coordinate Unit Vectors The body coordinate unit vectors are updated using the Newmark 𝛽-Method [Newmark 1959] with 𝛽 = 0, which is almost identical to the central difference method [Belytschko 1974]. In particular, the body component unit vectors are updated using the formula 𝑗+1 = 𝐛𝑖 𝐛𝑖 𝑗 + Δ𝑡 d𝐛𝑖 d𝑡 Δ𝑡2 d2𝐛𝑖 d𝑡2 , + (6.23) where the superscripts refer to the time step and the subscripts refer to the three unit vectors comprising the body coordinate triad. The time derivatives in the above equation are replaced by their equivalent forms from vector analysis: = 𝛚 × 𝐛𝑖 𝑗 d𝐛𝑖 d𝑡 𝑗 d2𝐛𝑖 d𝑡2 = 𝛚 × (𝛚 × 𝐛𝑖) + (𝛂𝑖 × 𝐛𝑖), (6.24) LS-DYNA Theory Manual Belytschko Beam where 𝜔 and 𝛼 are vectors of angular velocity and acceleration, respectively, obtained from the rotational equations of motion. With the above relations substituted into Equation (6.23), the update formula for the unit vectors becomes 𝑗+1 = 𝐛𝑖 𝐛𝑖 𝑗 + Δ𝑡(𝛚 × 𝐛𝑖) + Δ𝑡2 {[𝛚 × (𝛚 × 𝐛𝑖) + (𝛂𝑖 × 𝐛𝑖)]}. (6.25) To obtain the formulation for the updated components of the unit vectors, the body coordinate system is temporarily considered to be fixed and then the dot product of Equation (6.25) is formed with the unit vector to be updated. For example, to update the 𝑥̅ component of 𝐛3, the dot product of Equation (6.25), with 𝑖 = 3, is formed with b1, which can be simplified to the relation 𝑗+1 = 𝐛1 𝑏̅ 𝑥3 𝑗 ⋅ 𝐛3 𝑗+1 = Δ𝑡𝜔𝑦 𝑗 + Similarly, 𝑗+1 = 𝐛2 𝑏̅ 𝑦3 𝑗 ⋅ 𝐛3 𝑗+1 = Δ𝑡𝜔𝑥 𝑗 + 𝑗+1 = 𝐛1 𝑏̅ 𝑧3 𝑗 ⋅ 𝐛2 𝑗+1 = Δ𝑡𝜔𝑧 𝑗 + Δ𝑡2 Δ𝑡2 Δ𝑡2 (𝜔𝑥 𝑗𝜔𝑧 𝑗 + 𝛼𝑦 𝑗), (𝜔𝑦 𝑗𝜔𝑧 𝑗 + 𝛼𝑥 𝑗) (6.26) (6.27) (𝜔𝑥 𝑗𝜔𝑦 𝑗 + 𝛼𝑧 𝑗). 𝑗+1 are found by using normality and The remaining components 𝐛3 orthogonality, where it is assumed that the angular velocities w are small during a time 𝑗+1 is a step so that the quadratic terms in the update relations can be ignored. Since 𝐛3 unit vector, normality provides the relation 𝑗+1 and 𝐛1 𝑗+1 = √1 − (𝑏̅ 𝑏̅ 𝑧3 𝑗+1) 𝑥3 − (𝑏̅ 𝑗+1) 𝑦3 . Next, if it is assumed that 𝑏̅ 𝑗+1 ≈ 1, orthogonality yields 𝑥1 𝑗+1 = − 𝑏̅ 𝑧1 𝑗+1 + 𝑏̅ 𝑏̅ 𝑥3 𝑗+1 𝑦3 . 𝑗+1𝑏̅ 𝑦1 𝑗+1 𝑏̅ 𝑧3 The component 𝑏̅ 𝑗+1 is then found by enforcing normality: 𝑥1 𝑗+1 = √1 − (𝑏̅ 𝑏̅ 𝑥1 𝑗+1) 𝑦1 − (𝑏̅ 𝑗+1) 𝑧1 . (6.28) (6.29) (6.30) The updated components of 𝐛1 and 𝐛3 are defined relative to the body coordinates at time step 𝑗. To complete the update and define the transformation matrix, Equation (6.1), at time step 𝑗 + 1, the updated unit vectors 𝐛1 and 𝐛3 are transformed to the global coordinate system, using Equation (6.1) with [𝛌] defined at step 𝑗, and their vector cross product is used to form 𝐛2. LS-DYNA Theory Manual Hughes-Liu Beam 7 Hughes-Liu Beam The Hughes-Liu beam element formulation, based on the shell [Hughes and Liu 1981a, 1981b] discussed later, was the first beam element we implemented. It has several desirable qualities: • It is incrementally objective (rigid body rotations do not generate strains), allowing for the treatment of finite strains that occur in many practical applica- tions; • It is simple, which usually translates into computational efficiency and robust- ness • It is compatible with the brick elements, because the element is based on a degenerated brick element formulation; • It includes finite transverse shear strains. The added computations needed to retain this strain component, compare to those for the assumption of no trans- verse shear strain, are insignificant. 7.1 Geometry The Hughes-Liu beam element is based on a degeneration of the isoparametric 8- node solid element, an approach originated by Ahmad et al., [1970]. Recall the solid element isoparametric mapping of the biunit cube with, 𝐱(𝜉 , 𝜂, 𝜁 ) = ∑ 𝑁𝑎(𝜉 , 𝜂, 𝜁 )𝑥𝑎 𝑎=1 , 𝑁𝑎(𝜉 , 𝜂, 𝜁 ) = (1 + 𝜉𝑎𝜉 )(1 + 𝜂𝑎𝜂)(1 + 𝜁𝑎𝜁 ) , (7.1) (7.2) Hughes-Liu Beam LS-DYNA Theory Manual where 𝐱 is an arbitrary point in the element, (𝜉 , 𝜂, 𝜁 ) are the parametric coordinates, 𝐱𝑎 are the global nodal coordinates of node 𝑎, and 𝑁𝑎 are the element shape functions evaluated at node 𝑎, i.e., (𝜉𝑎, 𝜂𝑎, 𝜁𝑎) are (𝜉 , 𝜂, 𝜁 ) evaluated at node 𝑎. In the beam geometry, 𝜉 determines the location along the axis of the beam and the coordinate pair (𝜂, 𝜁 ) defines a point on the cross section. To degenerate the 8-node brick geometry into the 2-node beam geometry, the four nodes at 𝜉 = −1 and at 𝜉 = 1 are combined into a single node with three translational and three rotational degrees of freedom. Orthogonal, inextensible nodal fibers are defined at each node for treating the rotational degrees of freedom. Figure 7.1 shows a schematic of the biunit cube and the beam element. The mapping of the biunit cube into the beam element is separated into three parts: 𝐱(𝜉 , 𝜂, 𝜁 ) = 𝐱̅(𝜉 ) + 𝐗(𝜉 , 𝜂, 𝜁 ), = 𝐱̅(𝜉 ) + 𝐗𝜁 (𝜉 , 𝜁 ) + 𝐗𝜂(𝜉 , 𝜂), (7.3) where 𝐱̅ denotes a position vector to a point on the reference axis of the beam, and 𝐗𝜁 are position vectors at point 𝐱̅ on the axis that define the fiber directions through and 𝐗𝜂 Biunit Cube Beam Element +1 ζ¯ -1 Nodal fibers Top Surface z+ x+ x^ x¯ x^ x- Bottom Surface z- Figure 7.1. Hughes-Liu beam element. LS-DYNA Theory Manual Hughes-Liu Beam that point. In particular, , 𝐱̅(𝜉 ) = ∑ 𝑁𝑎(𝜉 )𝐱̅𝑎 𝑎=1 𝐗𝜂(𝜉 , 𝜂) = ∑ 𝑁𝑎(𝜉 )𝐗𝜂𝑎(𝜂) 𝑎=1 . 𝐗𝜁 (𝜉 , 𝜁 ) = ∑ 𝑁𝑎(𝜉 )𝐗𝜁𝑎(𝜁 ) 𝑎=1 , (7.4) With this description, arbitrary points on the reference line 𝐱̅ are interpolated by the one- dimensional shape function 𝑁(𝜉 ) operating on the global position of the two beam nodes that define the reference axis, i.e., 𝐱̅a. Points off the reference axis are further interpolated by using a one-dimensional shape function along the fiber directions, i.e., 𝐗𝜂𝑎(𝜂) and 𝐗𝜁𝑎(𝜁 ) where 𝐗𝜂𝑎(𝜂) = 𝑧𝜂𝑎(𝜂)𝐗̂𝜂𝑎 𝑧𝜂𝑎(𝜂) = 𝑁+(𝜂)𝑧𝜂𝑎 𝐗𝜁𝑎(𝜁 ) = 𝑧𝜁𝑎(𝜁 )𝐗̂𝜁𝑎 𝑧𝜁𝑎(𝜁 ) = 𝑁+(𝜁 )𝑧𝜁𝑎 − + + 𝑁−(𝜂)𝑧𝜂𝑎 + + 𝑁−(𝜁 )𝑧𝜁𝑎 − 𝑁+(𝜂) = 𝑁−(𝜂) = (1 + 𝜂) (1 − 𝜂) 𝑁+(𝜁 ) = 𝑁−(𝜁 ) = (1 + 𝜁 ) (1 − 𝜁 ) (7.5) where 𝑧𝜁 (𝜁 ) and 𝑧𝜂(𝜂) are “thickness functions”. The Hughes-Liu beam formulation uses four position vectors, in addition to 𝜉 , to locate the reference axis and define the initial fiber directions. Consider the two − located on the top and bottom surfaces, respectively, at position vectors 𝐱𝜁𝑎 node 𝑎. Then + and 𝐱𝜁𝑎 + , − + (1 + 𝜁 ̅)𝐱𝜁𝑎 , 𝐱̅𝜁𝑎 = 𝐗̂𝜁𝑎 = (1 − 𝜁 ̅)𝐱𝜁𝑎 + − 𝐱𝜁𝑎 − ) (𝐱𝜁𝑎 + − 𝐱𝜁𝑎 − ∥ ∥𝐱𝜁𝑎 (1 − 𝜁 ̅)∥𝐱𝜁𝑎 − = − 𝑧𝜁𝑎 + = 𝑧𝜁𝑎 + − 𝐱𝜁𝑎 − ∥, (1 + 𝜁 ̅)∥𝐱𝜁𝑎 + − 𝐱𝜁𝑎 − ∥, + , − + (1 + 𝜁 ̅)𝐱𝜂𝑎 𝐱̅𝜂𝑎 = 𝐗̂𝜂𝑎 = (1 − 𝜁 ̅)𝐱𝜂𝑎 + − 𝐱𝜂𝑎 − ) (𝐱𝜂𝑎 + − 𝐱𝜂𝑎 − ∥ ∥𝐱𝜂𝑎 − = − 𝑧𝜂𝑎 (1 − 𝜂̅)∥𝐱𝜂𝑎 + = 𝑧𝜂𝑎 , + − 𝐱𝜂𝑎 − ∥, (1 + 𝜂̅)∥𝐱𝜂𝑎 + − 𝐱𝜂𝑎 − ∥, (7.6) where ‖ ⋅ ‖ is the Euclidean norm. The reference surface may be located at the midsurface of the beam or offset at the outer surfaces. This capability is useful in several practical situations involving contact surfaces, connection of beam elements to solid elements, and offsetting elements such as for beam stiffeners in stiffened shells. The reference surfaces are located within the beam element by specifying the value of the parameters 𝜂̅ and 𝜁 ̅, . When these parameters take on the values –1 or +1, the reference axis is located on the outer surfaces of the beam. If they are set to zero, the reference axis is at the center. Hughes-Liu Beam LS-DYNA Theory Manual The same parametric representation used to describe the geometry of the beam elements is used to interpolate the beam element displacements, i.e., an isoparametric representation. Again the displacements are separated into the reference axis displacements and rotations associated with the fiber directions: 𝐮(𝜉 , 𝜂, 𝜁 ) = 𝐮̅̅̅̅(𝜉 ) + 𝐔(𝜉 , 𝜂, 𝜁 ), = 𝐮̅̅̅̅(𝜉 ) + 𝐔𝜁 (𝜉 , 𝜁 ) + 𝐔𝜂(𝜉 , 𝜂). The reference axis is interpolated as usual 𝐮̅̅̅̅(𝜉 ) = ∑ 𝑁𝑎(𝜉 )𝐮̅̅̅̅𝑎 𝑎=1 . The displacements are also interpolated along the reference axis 𝐔𝜂(𝜉 , 𝜂) = ∑ 𝑁𝑎(𝜉 )𝐔𝜂𝑎(𝜂), 𝑎=1 𝐔𝜁 (𝜉 , 𝜁 ) = ∑ 𝑁𝑎(𝜉 )𝐔𝜁𝑎(𝜁 ) 𝑎=1 . The fiber displacement is interpolated consistently with the thickness, 𝐔𝜂𝑎(𝜂) = 𝑧𝜂𝑎(𝜂)𝐔̂𝜂𝑎, 𝐔𝜁𝑎(𝜁 ) = 𝑧𝜁𝑎(𝜁 )𝐔̂𝜁𝑎, (7.7) (7.8) (7.9) (7.10) where 𝐮 is the displacement of a generic point, 𝐮̅̅̅̅ is the displacement of a point on the reference surface, and 𝑈 is the “fiber displacement” rotations. The motion of the fibers can be interpreted as either displacements or rotations as will be discussed. Hughes and Liu introduced the notation that follows, and the associated schematic shown in Figure 7.2, to describe the current deformed configuration with respect to the reference configuration. 𝐲 = 𝐲̅̅̅̅ + 𝐘, 𝐲̅̅̅̅ = 𝐱̅ + 𝐮̅̅̅̅, 𝐲̅̅̅̅𝑎 = 𝐱̅𝑎 + 𝐮̅̅̅̅𝑎, 𝐘 = 𝐗 + 𝐔, 𝐘𝑎 = 𝐗𝑎 + 𝐔𝑎, 𝐘̂𝜂𝑎 = 𝐗̂𝜂𝑎 + 𝐔̂𝜂𝑎, 𝐘̂𝜁𝑎 = 𝐗̂𝜁𝑎 + 𝐔̂𝜁𝑎, (7.11) In the above relations, and in Figure 7.2, the 𝐱 quantities refer to the reference configuration, the 𝐲 quantities refer to the updated (deformed) configuration and the 𝐮 quantities are the displacements. The notation consistently uses a superscript bar (⋅ ̅) to indicate reference surface quantities, a superscript caret (⋅ ̂) to indicate unit vector quantities, lower case letter for translational displacements, and upper case letters for fiber displacements. Thus to update to the deformed configuration, two vector quantities are needed: the reference surface displacement 𝐮̅̅̅̅ and the associated nodal fiber displacement 𝐔. The nodal fiber displacements are defined in the fiber coordinate system, described in the next subsection. LS-DYNA Theory Manual Hughes-Liu Beam (parallel construction) reference axis in undeformed geometry u¯ Deformed Configuration Reference Surface x¯ Figure 7.2. Schematic of deformed configuration displacements and position vectors. 7.2 Fiber Coordinate System For a beam element, the known quantities will be the displacements of the reference surface 𝑢̅ obtained from the translational equations of motion and the rotational quantities at each node obtained from the rotational equations of motion. What remains to complete the kinematics is a relation between nodal rotations and fiber displacements 𝐔. The linearized relationships between the incremental components Δ𝐔̂ the incremental rotations are given by ⎧Δ𝑈̂𝜂1 ⎫ }} {{ Δ𝑈̂𝜂2 ⎬ ⎨ }} {{ Δ𝑈̂𝜂3⎭ ⎩ ⎧Δ𝑈̂𝜁1 ⎫ }} {{ Δ𝑈̂𝜁2 ⎬ ⎨ }} {{ Δ𝑈̂𝜁3⎭ ⎩ = = ⎡ ⎢⎢⎢ −𝑌̂𝜂3 𝑌̂𝜂2 −𝑌̂𝜂1 ⎣ ⎡ ⎢⎢⎢ −𝑌̂𝜁3 𝑌̂𝜁2 −𝑌̂𝜁1 ⎣ 𝑌̂𝜂3 −𝑌̂𝜂2 ⎤ ⎥⎥⎥ 𝑌̂𝜂1 0 ⎦ 𝑌̂𝜁3 −𝑌̂𝜁2 ⎤ ⎥⎥⎥ 𝑌̂𝜁1 0 ⎦ {⎧Δ𝜃1 }⎫ Δ𝜃2 Δ𝜃3⎭}⎬ ⎩{⎨ {⎧Δ𝜃1 }⎫ Δ𝜃2 Δ𝜃3⎭}⎬ ⎩{⎨ = 𝐡𝜂Δ𝛉, = 𝐡𝜁 Δ𝛉. (7.12) Equations (7.12) are used to transform the incremental fiber tip displacements to rotational increments in the equations of motion. The second-order accurate rotational update formulation due to Hughes and Winget [1980] is used to update the fiber vectors: then LS-DYNA Draft 𝑌̂ 𝑌̂ 𝑛+1 = 𝑅𝑖𝑗(Δ𝜃)𝑌̂𝜂𝑖 𝑛, 𝜂𝑖 𝑛+1 = 𝑅𝑖𝑗(Δ𝜃)𝑌̂ 𝑛, 𝜁𝑖 𝜁𝑖 Hughes-Liu Beam LS-DYNA Theory Manual Δ𝐔̂𝜂𝑎 = 𝐘̂𝜂𝑎 Δ𝐔̂𝜁𝑎 = 𝐘̂ 𝑛+1 − 𝐘̂𝜂𝑎 𝑛 , 𝑛+1 − 𝐘̂𝜁𝑎 𝑛 , 𝜁𝑎 where 𝑅𝑖𝑗(Δ𝜃) = 𝛿𝑖𝑗 + (2𝛿𝑖𝑗 + Δ𝑆𝑖𝑘)Δ𝑆𝑖𝑘 2𝐷 Δ𝑆𝑖𝑗 = 𝑒𝑖𝑘𝑗Δ𝜃𝑘, , (7.14) (7.15) 2𝐷 = 2 + (Δ𝜃1 2 + Δ𝜃2 2 + Δ𝜃3 2). Here 𝛿𝑖𝑗 is the Kronecker delta and 𝑒𝑖𝑘𝑗 is the permutation tensor. 7.2.1 Local Coordinate System In addition to the above described fiber coordinate system, a local coordinate system is needed to enforce the zero normal stress conditions transverse to the axis. The orthonormal basis with two directions 𝐞̂2 and 𝐞̂3 normal to the axis of the beam is constructed as follows: 𝐞̂1 = 𝐞′2 = , 𝐲̅̅̅̅2 − 𝐲̅̅̅̅1 ∥𝐲̅̅̅̅2 − 𝐲̅̅̅̅1∥ 𝐘̂𝜂1 + 𝐘̂𝜂2 ∥𝐘̂𝜂1 + 𝐘̂𝜂2∥ . From the vector cross product of these local tangents. and to complete this orthonormal basis, the vector 𝐞̂3 = 𝐞̂1 × 𝐞′2, 𝐞̂2 = 𝐞̂3 × 𝐞̂1, (7.16) (7.17) (7.18) is defined. This coordinate system rigidly rotates with the deformations of the element. The transformation of vectors from the global to the local coordinate system can now be defined in terms of the basis vectors as 𝐀̂ = ⎧𝐴̂𝑥 ⎫ }} {{ 𝐴̂𝑦 ⎬ ⎨ }} {{ 𝐴̂𝑧⎭ ⎩ = 𝑒1𝑥 ⎢⎡ 𝑒1𝑦 𝑒1𝑧 ⎣ 𝑒2𝑥 𝑒2𝑦 𝑒2𝑧 𝑒3𝑥 ⎥⎤ 𝑒3𝑦 𝑒3𝑧⎦ {⎧𝐴𝑥 }⎫ 𝐴𝑦 𝐴𝑧⎭}⎬ ⎩{⎨ = [𝐪]{𝐀}, (7.19) where 𝑒𝑖𝑥, 𝑒𝑖𝑦, 𝑒𝑖𝑧 are the global components of the local coordinate unit vectors, 𝐀̂ is a vector in the local coordinates, and 𝐀 is the same vector in the global coordinate system. LS-DYNA Theory Manual Hughes-Liu Beam 7.3 Strains and Stress Update 7.3.1 Incremental Strain and Spin Tensors The strain and spin increments are calculated from the incremental displacement gradient 𝐺𝑖𝑗 = ∂Δ𝑢𝑖 ∂𝑦𝑗 , (7.20) where Δ𝑢𝑖 are the incremental displacements and 𝑦𝑗 are the deformed coordinates. The incremental strain and spin tensors are defined as the symmetric and skew-symmetric parts, respectively, of 𝐺𝑖𝑗: Δ𝜀𝑖𝑗 = Δ𝜔𝑖𝑗 = (𝐺𝑖𝑗 + 𝐺𝑗𝑖), (𝐺𝑖𝑗 − 𝐺𝑗𝑖). (7.21) The incremental spin tensor Δ𝜔𝑖𝑗 is used as an approximation to the rotational contribution of the Jaumann rate of the stress tensor; in an implicit implementation [Hallquist 1981b] the more accurate Hughes-Winget [1980] transformation matrix is used, Equation (7.15), with the incremental spin tensor for the rotational update. Here the Jaumann rate update is approximated as 𝜎 𝑖𝑗 = 𝜎𝑖𝑗 𝑛 + 𝜎𝑖𝑝 𝑛 Δ𝜔𝑝𝑗 + 𝜎𝑗𝑝 𝑛 Δ𝜔𝑝𝑖, (7.22) where the superscripts on the stress tensor refer to the updated (𝑛 + 1) and reference (𝑛) configurations. This update of the stress tensor is applied before the constitutive evaluation, and the stress and strain are stored in the global coordinate system. 7.3.2 Stress Update To evaluate the constitutive relation, the stresses and strain increments are rotated from the global to the local coordinate system using the transformation defined previously in Equation (7.19), viz. 𝑙𝑛 𝜎𝑖𝑗 Δ𝜀𝑖𝑗 = 𝑞𝑖𝑘𝜎 𝑘𝑛𝑞𝑗𝑛, 𝑙 = 𝑞𝑖𝑘Δ𝜀𝑘𝑛𝑞𝑗𝑛, (7.23) where the superscript 𝑙 indicates components in the local coordinate system. The stress is updated incrementally: 𝑙𝑛+1 𝜎𝑖𝑗 𝑙𝑛 = 𝜎𝑖𝑗 + Δ𝜎𝑖𝑗 𝑛+1 2, and rotated back to the global system: 𝑙𝑛+1 𝑛+1 = 𝑞𝑘𝑖𝜎𝑘𝑛 𝜎𝑖𝑗 𝑞𝑛𝑗, (7.24) (7.25) Hughes-Liu Beam LS-DYNA Theory Manual before computing the internal force vector. 7.3.3 Incremental Strain-Displacement Relations After the constitutive evaluation is completed, the fully updated stresses are rotated back to the global coordinate system. These global stresses are then used to update the internal force vector int = ∫ 𝐁𝑎 𝐟𝑎 T𝛔𝑑𝜐, (7.26) int are the internal forces at node 𝑎 and 𝐁𝑎 is the strain-displacement matrix in where 𝐟𝑎 the global coordinate system associated with the displacements at node 𝑎. The 𝐁 matrix relates six global strain components to eighteen incremental displacements [three translational displacements per node and the six incremental fiber tip displacements of Equation (7.14)]. It is convenient to partition the 𝐁 matrix: Each 𝐵𝑎 sub matrix is further partitioned into a portion due to strain and spin with the following sub matrix definitions: 𝐁 = [𝐁1, 𝐁2]. (7.27) 𝐵1 ⎡ 𝐵2 ⎢ ⎢ ⎢ ⎢ 𝐵2 𝐵1 ⎢ ⎢ 𝐵3 ⎣ 𝐵3 𝐵3 𝐵2 𝐵4 𝐵5 𝐵5 𝐵4 𝐵1 𝐵6 𝐵6 𝐵6 𝐵5 𝐵7 𝐵8 𝐵8 𝐵7 𝐵4 𝐵9 ⎤ ⎥ ⎥ 𝐵9 ⎥ , ⎥ ⎥ 𝐵9 𝐵8 ⎥ 𝐵7⎦ 𝐁𝑎 = where, 𝐵𝑖 = ⎧ { { { { { ⎨ { { { { { ⎩ 𝑁𝑎,𝑖 = (𝑁𝑎𝑧𝜂𝑎) ,𝑖−3 (𝑁𝑎𝑧𝜁𝑎) ,𝑖−6 = = 𝜕𝑁𝑎 𝜕𝑦𝑖 𝜕(𝑁𝑎𝑧𝜂𝑎) 𝜕𝑦𝑖−3 𝜕(𝑁𝑎𝑧𝜁𝑎) 𝜕𝑦𝑖−6 𝑖 = 1,2,3 𝑖 = 4,5,6 . 𝑖 = 7,8,9 (7.28) (7.29) With respect to the strain-displacement relations, note that: • The derivative of the shape functions are taken with respect to the global coordinates; • The 𝐁 matrix is computed on the cross-section located at the mid-point of the axis; • The resulting 𝐁 matrix is a 6 × 18 matrix. The internal force, 𝑓 , given by int 𝐟′ = 𝐓T𝐟𝑎 7-8 (Hughes-Liu Beam) LS-DYNA Theory Manual Hughes-Liu Beam 11 12 10 16 13 15 14 Figure 7.3. Integration possibilities for rectangular cross sections in the Hughes-Liu beam element. is assembled into the global right hand side internal force vector. 𝐓 is defined as (also see Equation (7.12): 𝐓 = ⎤ ⎡ 𝟎 𝐡𝜂 , ⎥ ⎢ 𝟎 𝐡𝜁 ⎦ ⎣ (7.31) where 𝐈 the 3 × 3 identity matrix. 7.3.4 Spatial Integration The integration of Equation (7.26) for the beam element is performed with one- point integration along the axis and multiple points in the cross section. For rectangular cross sections, a variety of choices are available as is shown in Figure 7.3. The beam has no zero energy or locking modes. Hughes-Liu Beam LS-DYNA Theory Manual st tt Figure 7.4. Specification of the nodal thickness, 𝑠𝑡 and 𝑡𝑡, for a beam with an arbitrary cross-section. For the user defined rule, it is necessary to specify the number of integration points and the relative area for the total cross section: 𝐴𝑟 = 𝐬𝑡 ⋅ 𝐭𝑡 where 𝑠𝑡 and 𝑡𝑡 are the beam thickness specified on either the cross section or beam element cards. The rectangular cross-section which contains 𝑠𝑡 and 𝑡𝑡 should completely contain the cross-sectional geometry. Figure 7.4 illustrates this for a typical cross- section. In Figure 5.5, the area is broken into twelve integration points. For each integration point, it is necessary to define the 𝑠 and 𝑡 parametric coordinates, (𝑠𝑖,𝑡𝑖), of the centroid of the ith integration point and the relative area associated with the point 𝐴𝑟𝑖 = 𝐴𝑖 LS-DYNA Theory Manual Hughes-Liu Beam A1 A2 A3 A4 A5 s6 A12 A11 A10 t6 A6 A7 A8 A9 Figure 7.5. A breakdown of the cross section geometry in Figure 7.4 into twelve integration points. where 𝐴𝑖 is the ratio of the area of the integration point and the actual area of the cross- section, 𝐴. LS-DYNA Theory Manual Warped Beam Elements 8 Warped Beam Elements 8.1 Resultant Warped Beam 8.1.1 Green-Lagrange Strains in Terms of Deformational Displacements All quantities in this section are referred to the local element coordinate system 𝐞𝑖, 𝑖 = 1, 2, 3. The origin of the local system is taken at node 1, with 𝐞1 directed along the line of centroids, while 𝐞2, and 𝐞3 are directed along the principal axes of the cross- section. With respect to the local system, the Green-Lagrange strain tensor can be written as: where, 𝜀𝑖𝑗 = 𝑒𝑖𝑗 + 𝜂𝑖𝑗, 𝑒𝑖𝑗 = 0.5(𝑢𝑖,𝑗 + 𝑢𝑗,𝑖), 𝜂𝑖𝑗 = 0.5𝑢𝑘,𝑖𝑢𝑘,𝑗. (8.1) (8.2) The geometric assumption of infinite in-plane rigidity implies 𝜀22 = 𝜀33 = 𝛾23 = 0. Then the non-zero strain components which contribute to the strain energy are: 2 + 𝑢2,1 2 + 𝑢3,1 (𝑢1,1 𝜀11 = 𝑢1,1 + 2𝜀12 = 𝑢1,2 + 𝑢2,1 + 𝑢1,1,𝑢1,2 + 𝑢2,1𝑢2,2 + 𝑢3,1𝑢3,2, 2𝜀13 = 𝑢1,3 + 𝑢3,1 + 𝑢1,1𝑢1,3 + 𝑢2,1𝑢2,3 + 𝑢3,1𝑢3,3. 2 ), (8.3) 8.1.2 Deformational Displacements After Large Rotations The position vectors of an arbitrary point P in the initial and current local configurations are: Warped Beam Elements LS-DYNA Theory Manual 0 = 𝐱𝐶 𝐱𝑃 0 + [𝐞1 𝐞2 𝐞3] ⎤, 𝑥2 ⎥ 𝑥3⎦ ⎡ ⎢ ⎣ 𝐱𝑃 = 𝐱𝐶 + [𝐞′1 𝐞′2 𝐞′3] 𝜛𝜙 ⎤, ⎡ 𝑥2 ⎥ ⎢ 𝑥3 ⎦ ⎣ respectively, with where [𝐞′1 𝐞′2 𝐞′3] = [𝐈 + 𝛉 + 𝛉2] [𝐞1 𝐞2 𝐞3], (8.4) (8.5) (8.6) −𝜃3 𝜃1 and 𝜛 is the Saint-Venant warping function about the centroid C. By the transfer theorem, the following relation holds: 𝜃2 ⎤ −𝜃1 , ⎥ 0 ⎦ ⎡ 𝜃3 ⎢ −𝜃2 ⎣ 𝛉 = (8.7) where 𝜔 refers to the shear center S, and 𝑐2 and 𝑐3 are the coordinates of S. 𝜛 = 𝜔 + 𝑐2𝑥3 − 𝑐3𝑥2, (8.8) Subtracting Equation (8.4) from Equation (8.5) and neglecting third-order terms, the displacements vector of point P can be computed: 𝑢1 = 𝑢̅1 − 𝑥2𝜃3 + 𝑥3𝜃2 + 𝑢2 = 𝑢̅2 − 𝑥3𝜃1 − u3 = u̅̅̅̅3 + x2θ1 − 2 + 𝜃3 2) + 𝑥2𝜃1𝜃2 + 2) + x3(θ1 2 + θ2 𝑥2(𝜃1 𝑥3𝜃1𝜃3 + 𝜛𝜙, 𝑥3𝜃2θ3 + 𝜛θ3𝜙, x2θ2θ3 − 𝜛θ2𝜙, (8.9) where 𝑢̅1, 𝑢̅2, and 𝑢̅3 are the displacements of the centroid C. 8.1.3 Green-Lagrange Strains in terms of Centroidal Displacements and Angular Rotations From Equations (8.3) and (8.9), a second-order approximation of the Green- 2 and the nonlinear strain Lagrange strains can be evaluated. Neglecting term 1 components generated by warping, the strain components are simplified as 2 𝑢1,1 𝜀11 = 𝜀0 + 𝑥2𝜅2 + 𝑥3𝜅3 + 2𝜀12 = 𝛾12 + 𝜛,2𝜙 − 𝑥3𝜅1, 2𝜀13 = 𝛾13 + 𝜛,3𝜙 + 𝑥2𝜅1, with (𝑥2 2 + 𝑥3 2)𝜃1,1 2 + 𝜔𝜙,1, (8.10) LS-DYNA Theory Manual Warped Beam Elements 𝜀0 = 𝑢̅1,1 + 𝜅1 = 𝜃1,1 + 𝜅2 = −𝜃3,1 + 𝜅3 = 𝜃2,1 + (𝑢̅2,1 2 + 𝑢̅3,1 2 ), (𝜃2,1𝜃3 − 𝜃3,1𝜃2), (𝜃1𝜃2,1 + 𝜃1,1𝜃2) + 𝑢̅3,1𝜃1,1 − 𝑐3𝜙,1, (𝜃1𝜃3,1 + 𝜃1,1𝜃3) − 𝑢̅2,1𝜃1,1 + 𝑐2𝜙,1, (8.11) 𝛾12 = 𝑢̅2,1 − 𝜃3 + 𝛾13 = 𝑢̅3,1 + 𝜃2 + 𝜃1𝜃2 + 𝑢̅3,1𝜃1 − 𝑢̅1,1𝜃3, 𝜃1𝜃3 − 𝑢̅2,1𝜃1 + 𝑢̅1,1𝜃2. Numerical testing has shown that neglecting the nonlinear terms in the curvatures 𝜅1, 𝜅2, 𝜅3 and bending shear strains 𝛾12, 𝛾13 has little effect on the accuracy of the results. Therefore, Equation (8.11) can be simplified to 𝜅1 = 𝜃1,1, 𝜀0 = 𝑢̅1,1 + 𝜅2 = −𝜃3,1 − 𝑐3𝜙,1, 𝜅3 = 𝜃2,1 + 𝑐2𝜙,1, (𝑢̅2,1 2 + 𝑢̅3,1 2 ), 𝛾12 = 𝑢̅2,1 − 𝜃3, 𝛾13 = 𝑢̅3,1 + 𝜃2. (8.12) Adopting Bernoulli’s assumption (𝛾12 = 𝛾13 = 0) and Vlasov’s assumption (𝜙 = θ1,1), Equation (8.10) can be rewritten as: 𝜀11 = 𝜀0 + 𝑥2𝜅2 + 𝑥3𝜅3 + 2𝜀12 = (𝜛,2 − 𝑥3)𝜅1, 2𝜀13 = (𝜛,3 − 𝑥2)𝜅1, 𝑟2𝜅1 2 + 𝜔𝜃1,11, where 𝑟2 = 𝑥2 2 + 𝑥3 2, 𝜅1 = 𝜃1,1, 𝜅2 = −𝑢̅2,11 − 𝑐3𝜃1,11, 𝜅3 = −𝑢̅3,11 + 𝑐2𝜃1,11. To avoid membrane locking, ε11 in Equation (8.13) is reformulated as 𝜀11 = 𝜀𝑎 + 𝑥2𝜅2 + 𝑥3𝜅3 + 2 + 𝜔𝜃1,11, (𝑟2 − ) 𝜅1 𝐼𝑜 where 𝜀𝑎 = ∫ [𝑢̅1,1 + 8.1.4 Strain Energy (𝑢̅2,1 2 + 𝑢̅3,1 2 + 𝐼𝑜 2)] 𝑑𝑥1 𝜅1 . (8.13) (8.14) (8.15) (8.16) Assuming material is linear elastic, the strain energy can be evaluated from: 2 𝑑𝐴 ∫ 𝜀11 with Warped Beam Elements LS-DYNA Theory Manual 𝑈 = ∫ ( 2 𝑑𝐴 + 𝐸 ∫ 𝜀11 𝐺 ∫ [(2𝜀12)2 + (2𝜀13)2]𝑑𝐴 ) 𝑑𝑥1. (8.17) The following relations are used in integrating the previous equations: (1) Since the reference frame is located at centroid C with e2 and e3 directed along the principal axes, ∫ 𝑥2𝑑𝐴 = 0 , ∫ 𝑥3𝑑𝐴 = 0 , ∫ 𝑥2𝑥3𝑑𝐴 = 0 . (2) Since sectorial area ω refers to shear center S, ∫ 𝜔𝑑𝐴 = 0 , ∫ 𝑥2𝜔𝑑𝐴 = 0 , ∫ 𝑥3𝜔𝑑𝐴 = 0 . Integration through the cross-section gives: + 𝐴𝜀𝑎 2 + 𝐼22𝜅2 2 + 𝐼𝜔𝜃1,11 2 + 𝐼2𝑟𝜅2𝜅1 2 + 𝐼3𝑟𝜅3𝜅1 2 + 𝐼𝜔𝑟𝜃1,11𝜅1 2 + 𝐼33𝜅3 𝐼𝑜 4 ) 𝜅1 + (𝐼𝑟𝑟 − ∫ [(2ε12)2 + (2ε13)2] 2 dA = 𝐽κ1 𝐼33 = ∫ 𝑥3 2𝑑𝐴 , 𝐼3𝑟 = ∫ 𝑥3𝑟2𝑑𝐴, 𝐼𝜔𝑟 = ∫ 𝜔𝑟2𝑑𝐴 , 𝐼𝑂 = 𝐼22 + 𝐼33 𝐼𝑟𝑟 = ∫ 𝑟4𝑑𝐴 𝐽 = ∫ [(𝜔̅̅̅̅,3 + 𝑥2)2 + (𝜔̅̅̅̅,2 − 𝑥3)2] 𝑑𝐴 𝐼22 = ∫ 𝑥2 2𝑑𝐴 , 𝐼2𝑟 = ∫ 𝑥2𝑟2𝑑𝐴, 𝐼𝜔 = ∫ 𝜔2𝑑𝐴 , 6.1.5 Displacement Field Linear interpolation is used for axial displacement 𝐮̅̅̅̅, whereas Hermitian interpolations are used for 𝑢2, 𝑢3, and 𝜃1, considering the following relations used in deriving the final expression of strain energy: 𝜃2 = −𝑢3,1 𝜃3 = 𝑢2,1 𝜙 = 𝜃1,1. The nodal displacement field is constructed by 𝑢̅1 = 𝐍1𝐝, (8.23) (8.24) 8-4 (Warped Beam Elements) LS-DYNA Draft (8.18) (8.19) (8.20) LS-DYNA Theory Manual Warped Beam Elements {⎧𝑢̅2 }⎫ 𝑢̅3 𝜃1 ⎭}⎬ ⎩{⎨ = 𝐍2𝐝, (8.25) where 𝐝T = [0 𝜃2𝐼 𝜃3𝐼 𝜙𝐼 𝑢̅1𝐽𝐼 𝜃1𝐽𝐼 𝜃2𝐽 𝜃3𝐽 𝜙𝐽]T, (8.26) 𝐍1 = [1 − 𝜉 ⋅⋅⋅⋅⋅⋅| 𝜉 ⋅ ⋅ ⋅ ∣ ⋅ 1 − 𝑓 ⋅ ⋅ ⋅ ℎ ⋅ ⋅ 𝑓 ⋅ ⋅ ⋅ 𝑔 ⋅ ∣∣∣ ⋅ ⋅ 1 − 𝑓 ⋅ −ℎ ⋅ ⋅ ⋅⋅ 𝑓 ⋅ −𝑔 ⋅ ⋅ ⋅ ⋅⋅ ⋅ 𝑓 ⋅ ⋅ 𝑔∣ 1 − 𝑓 ⋅ ], ⋅ ⋅ ⋅ ⋅ ⋅ 𝐍2 = ⎡ ⎢ ⎣ with 𝑓 = 1 − 3𝜉 2 + 2𝜉 3𝑔 = 𝑙(𝜉 − 2𝜉 2 + 𝜉 3)ℎ = 𝑙(𝜉 3 − 𝜉 2). Equations (8.25) and (8.27) also imply 𝜃1,1 = 𝐍3𝐝, where 𝐍3 = [⋅⋅ 𝑓,1 ⋅⋅ 𝑔,1∣ ⋅⋅⋅ −𝑓,1 ⋅⋅ ℎ,1]. ⎤ , ⎥ ⋅ ℎ⎦ (8.27) (8.28) (8.29) (8.30) 6.1.6 Strain Energy in Matrix Form The strain energy due to the average strain εa defined in Equation (8.16) can be expressed in matrix form as 𝑈1 = where 𝐸𝐴𝑙 [∫ (𝐍1,1𝐝)𝑑𝜉 + 𝐝T [∫ (𝐍2,1 T 𝐃𝐍2,1)𝑑𝜉 ] 𝐝 ] , 𝐃 = diag (1,1, 𝐼𝑜 ). The strain energy due to the second through fourth terms is 𝑈2 = 𝐸𝑙𝐝T [∫ 𝐍2,11 T 𝐇𝐍2,11𝑑𝜉 ] 𝐝, (8.31) (8.32) (8.33) where 𝐇 = 𝐼22 ⎡ ⎢ 𝐼22𝑐3 −𝐼33𝑐2 ⎣ 𝐼33 𝐼22𝑐3 −𝐼33𝑐2 𝐼′𝜔 ⎤ ⎥ ⎦ , 𝐼′𝜔 = 𝐼𝜔 + 𝐼22𝑐3 2. 2 + 𝐼33𝑐2 (8.34) The strain energy due to the fifth through seventh terms is Warped Beam Elements LS-DYNA Theory Manual 𝑈3 = 𝐸𝑙 [∫ (𝐍3𝐝)2 𝛖𝐍2,11𝑑𝜉 ] 𝐝, where 𝛖 = (−𝐼2𝑟 − 𝐼3𝑟 𝐼′𝜔𝑟), 𝐼′𝜔𝑟 = 𝐼𝜔𝑟 − 𝑐3𝐼2𝑟 + 𝑐2𝐼3𝑟. The strain energy due to the eighth and ninth terms is 𝑈4 = 𝐸𝑙 (𝐼𝑟𝑟 − 𝐼𝑜 ) ∫ (𝐍3𝐝)4𝑑𝜉 + 𝐺𝐽𝑙 ∫ (𝐍3𝐝)2𝑑𝜉 (8.35) (8.36) (8.37) 6.1.7 Internal Nodal Force Vector The internal force can be evaluated from 𝐟e = 𝐸𝐴𝑙 ( 𝐮̅̅̅̅1𝐽𝐿 + 𝐝T𝐐) (𝐏 + 𝐐) + 𝐸 (𝐑 + 𝐒 + 𝐓 + 𝐕) + G𝐖, (8.38) where 𝐏 = ∫ 𝐍1,1 T 𝑑𝜉 , 𝐐 = [∫ 𝐍2,1 𝐒 = l [∫ (𝐍3𝐝)2 𝐍2,11 T 𝑑𝜉 ] 𝛖T, 𝐓 = 𝑙 ∫ (𝐍3𝐝)(𝛖𝐍2,11𝐝) 𝐃𝐍2,1𝑑𝜉 ] 𝐝, T 𝐇𝐍2,11𝑑𝜉 𝐑 = l [∫ 𝐍2,11 T𝑑𝜉 , 𝐍3 ] 𝐝, (8.39) 𝐕 = (𝐼𝑟𝑟 − 𝐼𝑜 ) l ∫ (𝐍3𝐝)3𝐍3 T𝑑𝜉 , 𝐖 = 𝐽𝑙 ∫ (𝐍3𝐝)𝐍3 T𝑑𝜉 , 𝜆 = 𝑢̅1𝐽𝐼 + 𝐝T𝐐. With respect to the local coordinate system, there are totally eight independent components in the nodal force vector, in correspondence to the eight nodal displacement components. Other forces can be calculated by: 𝐅1 = −𝐅8, 𝐅2 = 𝐅4 = −𝐅11, 𝐅9 = −𝐅2, 𝐅6 + 𝐅13 , 𝐅5 + 𝐅12 𝐅3 = − 𝐅10 = −𝐅3. , (8.40) 6.2 Integrated Warped Beam 6.2.1 Kinematics We introduce three coordinate systems that are mutually interrelated. The first coordinate system is the orthogonal Cartesian coordinate system (𝑥, 𝑦, 𝑧), for which the y and zaxes lie in the plane of the cross-section and the 𝑥-axis parallel to the longitudinal axis of the beam. The second coordinate system is the local plate coordinate system (𝑥, 𝑠, 𝑛) as shown in Figure 6.1, wherein the n-axis is normal to the middle surface of a plate element, the s-axis is tangent to the middle surface and is directed along the contour line of the cross-section. The (𝑥, 𝑠, 𝑛) and (𝑥, 𝑦, 𝑧) coordinate LS-DYNA Theory Manual Warped Beam Elements systems are related through an angle of orientation 𝜃 as defined in Figure 40.1. The third coordinate set is the contour coordinate s along the profile of the section with its origin at some point O on the profile section. Point P is called the pole through which the axis parallel to the x-axis is called the pole axis. To derive the analytical model for a thin- walled beam, the following two assumptions are made: 1. The contour of the thin wall does not deform in its own plane. 2. The shear strain γsx of the middle surface is zero. According to assumption 1, the midsurface displacement components 𝑣 and 𝑤 with respect to the (𝑥, 𝑠, 𝑛) coordinate system at a point A can be expressed in terms of displacements 𝐕 and 𝐖 of the pole P in the (𝑥, 𝑦, 𝑧) coordinate system and the rotation angle 𝜙𝑥 about the pole axis 𝐯(𝑥, 𝑠) = 𝐕(𝑥)cos𝜃(𝑠) + 𝐖(𝑥)sin𝜃(𝑠) − 𝐫(𝑠)ϕ𝑥(𝑥), 𝐰(𝑥, 𝑠) = −𝐕(𝑥)sin𝜃(𝑠) + 𝐖(𝑥)cos𝜃(𝑠) − 𝐪(𝑠)ϕ𝑥(𝑥). (8.41) These equations apply to the whole contour. The out-of-plane displacement u can now be found from assumption 2. On the middle surface ∂𝐮 ∂𝑠 + ∂𝐯 ∂𝑥 = 𝟎, which can be written ∂𝐮 ∂s = − ∂𝐯 ∂𝑥 = −𝐕′(𝑥)cos𝜃(𝑠) − 𝐖′(𝑥)sin𝜃(𝑠) + 𝐫(𝑠)ϕ′𝑥(𝑥). (8.42) (8.43) Integrating this relation from point O to an arbitrary point on the contour yields (using t as a dummy for s) q(s) θ(s) r(s) Figure 8.1. Definition of coordinates in thin-walled open section Warped Beam Elements LS-DYNA Theory Manual ∫ ∂𝐮 ∂𝑡 𝑑𝑡 = −𝐕′(𝑥) ∫ cos𝜃(𝑡)𝑑𝑡 − 𝐖′(𝑥) ∫ sin𝜃(𝑡)𝑑𝑡 + ϕ′𝑥(𝑥) ∫ 𝐫(𝑡)𝑑𝑡 . Noting that we end up with 𝑑𝑦 = cos𝜃(𝑡)𝑑𝑡, 𝑑𝑧 = sin𝜃(𝑡)𝑑𝑡. 𝑢(𝑥, 𝑠) = 𝑢(𝑥, 0) + V′(𝑥)𝑦(0) + W′(𝑥)𝑧(0) + ϕ′𝑥(𝑥)ϖ ⏟⏟⏟⏟⏟⏟⏟⏟⏟⏟⏟⏟⏟⏟⏟⏟⏟⏟⏟⏟⏟⏟⏟ =:𝐔(𝑥) − 𝑉′(𝑥)⏟ =:𝜙𝑧(𝑥) 𝑦(𝑠) − W′(𝑥)⏟ =:−𝜙𝑦(𝑥) = 𝑈(𝑥) − 𝜙𝑧(𝑥)𝑦 + 𝜙𝑦(𝑥)𝑧 + 𝜙′𝑥(𝑥)(𝜔(𝑠) − ϖ). z(𝑠) + ϕ′𝑥(𝑥)(ω(𝑠) − ϖ) (8.44) (8.45) (8.46) where 𝑈 denotes the average out-of-plane displacement over the section, 𝜙𝑦 and 𝜙𝑧 denote the rotation angle about the y and z axis1, respectively, ω is the sectorial area defined as 𝜔(𝑠) = ∫ 𝑟(𝑡)𝑑𝑡 , and ϖ is the average of the sectorial area over the section. The expression for the displacements in the (x, y, z) coordinate system is 𝑢(𝑥, 𝑦, 𝑧) = 𝑈(𝑥) − 𝜙𝑧(𝑥)𝑦 + 𝜙𝑦(𝑥)𝑧 + 𝜗(𝑥)𝜔(𝑦, 𝑧), 𝑣(𝑥, 𝑦, 𝑧) = 𝑉(𝑥) − 𝜙𝑥(𝑥)𝑧, 𝑤(𝑥, 𝑦, 𝑧) = 𝑊(𝑥) + 𝜙𝑥(𝑥)𝑦, where we have introduced ϑ to represent the twist constrained by the condition 𝜗(𝑥) = 𝜙𝑥(𝑥). (8.47) (8.48) (8.49) and 𝜔 denotes the sectorial coordinate that is adjusted for zero average over the section. 6.2.2 Kinetics The kinetic energy of the beam can be written 𝑇 = ∫ 𝜌{𝑢̇2 + 𝑣̇2 + 𝑤̇ 2} 𝑑𝑉. (8.50) Taking the variation of this expression leads to 1 The substitution of 𝑉′(𝑥) for 𝜙(cid:3053)(𝑥) and 𝑊′(𝑥) for −𝜙(cid:3052)(𝑥) can be seen as a conversion from an Euler- Bernoulli kinematic assumption to that of Timoschenko. LS-DYNA Theory Manual Warped Beam Elements δT = ∫ ρ{u̇δu̇ + v̇δv̇ + ẇ δẇ } dV = ∫ ρ{U̇ − 𝜙̇zy + 𝜙̇yz + 𝜗̇ω}{δU̇ − δ𝜙̇zy + δ𝜙̇yz + δ𝜗̇ω}dV + ∫ ρ{V̇ − 𝜙̇xz}{δV̇ − δ𝜙̇xz}dV + ∫ ρ{Ẇ + 𝜙̇xy}{δẆ + δ𝜙̇xy}dV = ∫ ρ{U̇ δU̇ + y2𝜙̇zδ𝜙̇z − yω𝜙̇zδ𝜗̇ + z2𝜙̇yδ𝜙̇y}dV + ∫ ρ{zω𝜙̇yδ𝜗̇ − yω𝜗̇δ𝜙̇z + zω𝜗̇δ𝜙̇y + ω2𝜗̇δ𝜗̇}dV + (8.51) ∫ ρ{V̇ δV̇ + z2𝜙̇xδ𝜙̇x + Ẇ δẆ + y2𝜙̇xδ𝜙̇x}dV = ρA ∫{U̇ δU̇ + V̇ δV̇ + Ẇ δẆ }dV + ρIzz ∫{𝜙̇zδ𝜙̇z + 𝜙̇xδ𝜙̇x}dV + ρIýy ∫{𝜙̇yδ𝜙̇y + 𝜙̇xδ𝜙̇x}dV + ρIyω ∫{𝜙̇yδ𝜗̇ + 𝜗̇δ𝜙̇y}dV − ρIzω ∫{𝜗̇δ𝜙̇z + 𝜙̇zδ𝜗̇}dV + ρIωω ∫ 𝜗̇δ𝜗̇dV , from which the consistent mass matrix can be read out. Here A is the cross sectional area, Izz and Iyy are the second moments of area with respect to the z and y axes, respectively, Iωω is the sectorial second moment and Izω and Iyω are the sectorial product moments. An approximation of this mass matrix can be made by neglecting the off diagonal components. The diagonal components are 𝑚TRNS = 𝜌𝐴𝑙 , , (8.52) 𝜌(𝐼𝑦𝑦 + 𝐼𝑧𝑧)𝑙 𝑚RT𝑥 = 𝑚RT𝑦 = 𝑚RT𝑧 = 𝑚TWST = , 𝜌𝐼𝑦𝑦𝑙 𝜌𝐼𝑧𝑧𝑙 𝜌𝐼𝜔𝜔𝑙 , . With 𝐸 as Young’s modulus and 𝐺 as the shear modulus, the strain energy can be written Warped Beam Elements LS-DYNA Theory Manual 𝛱 = (𝐸𝜀𝑥𝑥 2 + 𝐺𝛾𝑥𝑦 2 + 𝐺𝛾𝑥𝑧 2 ), (8.53) where the infinitesimal strain components are (neglecting the derivatives of sectorial area) ′ 𝑦 + 𝜗′𝜔, 𝜀𝑥𝑥 = 𝑈′ + 𝜙𝑦 𝛾𝑥𝑦 = 𝑉′ − 𝜙𝑥 𝛾𝑥𝑧 = 𝑊′ + 𝜙𝑥 ′ 𝑧 − 𝜙𝑧 ′ 𝑧 − 𝜙𝑧, ′ 𝑦 + 𝜙𝑦. and the variation of the same can be written 𝛿𝜀𝑥𝑥 = 𝛿𝑈′ + 𝛿𝜙𝑦 𝛿𝛾𝑥𝑦 = 𝛿𝑉′ − 𝛿𝜙𝑥 𝛿𝛾𝑥𝑧 = 𝛿𝑊′ + 𝛿𝜙𝑥 ′ 𝑧 − 𝛿𝜙𝑧 ′ 𝑧 − 𝛿𝜙𝑧, ′ 𝑦 + 𝛿𝜙𝑦. ′ 𝑦 + 𝛿𝜗′𝜔, The variation of the strain energy is 𝛿𝛱 = ∫{𝐸𝜀𝑥𝑥𝛿𝜀𝑥𝑥 + 𝐺𝛾𝑥𝑦𝛿𝛾𝑥𝑦 + 𝐺𝛾𝑥𝑧𝛿𝛾𝑥𝑧}𝑑𝑉 = 𝐸𝐴 ∫ 𝑈′𝛿𝑈′𝑑𝑙 + 𝐺𝐴 ∫ 𝑉′𝛿𝑉′𝑑𝑙 𝐸𝐼𝑦𝑦 ∫ 𝜙𝑦 ′ 𝛿𝜙𝑦 ′ 𝑑𝑙 + 𝐺𝐴 ∫ 𝜙𝑦𝛿𝜙𝑦𝑑𝑙 𝐸𝐼𝜔𝜔 ∫ 𝜗′𝛿𝜗′𝑑𝑙 − 𝐺𝐴 ∫(𝑉′𝛿𝜙𝑧 + 𝜙𝑧𝛿𝑉′)𝑑𝑙 + 𝐺𝐴 ∫ 𝑊′𝛿𝑊′𝑑𝑙 + 𝐺(𝐼𝑦𝑦 + 𝐼𝑧𝑧) ∫ 𝜙𝑥 ′ 𝛿𝜙𝑥 ′ 𝑑𝑙 + 𝐸𝐼𝑧𝑧 ∫ 𝜙𝑧 ′ 𝑑𝑙 ′ 𝛿𝜙𝑧 + 𝐺𝐴 ∫ 𝜙𝑧𝛿𝜙𝑧𝑑𝑙 + 𝐺𝐴 ∫(𝑊′𝛿𝜙𝑦 + 𝜙𝑦𝛿𝑊′)𝑑𝑙 + + (8.54) (8.55) + (8.56) 𝐸𝐼𝑦𝜔 ∫(𝜙𝑦 ′ )𝑑𝑙 ′ 𝛿𝜗′ + 𝜗′𝛿𝜙𝑦 − 𝐸𝐼𝑧𝜔 ∫(𝜙𝑧 ′ 𝛿𝜗′ + 𝜗′𝛿𝜙𝑧 ′ )𝑑𝑙 , where the stiffness matrix can be read. Again the diagonal components are LS-DYNA Theory Manual Warped Beam Elements 𝑘TRNS = 𝑘SHR = 𝑘RTx = 𝑘RTy = 𝑘RTz = , 𝐸𝐴 𝐺𝐴 , 𝐺(𝐼𝑦𝑦 + 𝐼𝑧𝑧) 𝐺𝐴𝑙 𝐺𝐴𝑙 , , + 𝐸𝐼𝑦𝑦 𝐸𝐼𝑧𝑧 + 𝐸𝐼𝜔𝜔 𝑘TWST = . , (8.57) From the expressions of the mass and stiffness matrix, the frequencies of the most common modes can be estimated. These are 1. The tensile and twisting modes with frequency 𝜔 = √3 √𝐸 𝜌. 2. The transverse shear and torsional mode with frequency 𝜔 = 3. The bending modes with frequencies 𝜔 = √3𝐸 𝜌𝑙2 + 𝐺𝐴 𝜌𝐼𝑦𝑦 and 𝜔 = √3𝐸 √3 √𝐺 𝜌. 𝜌𝑙2 + 𝐺𝐴 𝜌𝐼𝑧𝑧 . Which one of these four that is the highest depends on the geometry of the beam element. In LS-DYNA the first of these frequencies is used for calculating a stable time step. We have found no reason for changing approach regarding this element. 6.2.3 Penalty on Twist The twist is constrained using a penalty that is introduced in the strain energy as 𝛱P = 𝑃𝐸A ′ − 𝜗)2𝑑𝑙 ∫(𝜙𝑥 , and the corresponding variation is 𝛿𝛱 = 𝑃𝐸𝐴 ∫(𝜙𝑥 ′ − 𝜗)(𝛿𝜙𝑥 ′ − 𝛿𝜗)𝑑𝑙 (8.58) (8.59) . The diagonal of the stiffness matrix is modified as follows Warped Beam Elements LS-DYNA Theory Manual 𝑘RTx = 𝑘TWST = + 𝐺(𝐼𝑦𝑦 + 𝐼𝑧𝑧) 𝐸𝐼𝜔𝜔 + 𝑃𝐸𝐴𝑙 𝑃𝐸𝐴 , . (8.60) This increases the twist mode frequency to √3𝐸 𝜌𝑙2 + 𝑃𝐸𝐴 𝜌𝐼𝜔𝜔 and the torsional mode to √3 √ 𝐺(𝐼𝑦𝑦 + 𝐼𝑧𝑧) + 𝑃𝐸𝐴 . (8.61) Even though this gives an indication of a frequency increase we have made no modifications on the computation of the critical time step in an explicit analysis. We have used 𝑃 = 1 in the implementation. This decision may have to be reconsidered depending on the choice of the parameter 𝜇, in the end it will come down to trial and error from numerical simulations. 6.3 Generalization to Large Displacements A generalization of the small displacement theory to nonlinear theory is quite straightforward. We have used a corotational formulation where the small strains in the linear theory are used directly as strain rates in the element system. We emphasize that the nonlinear beam formulation is obtained by simply replacing displacements for velocities and strains with strain rates in the previous section. The nodal velocities for a beam element in the local system is written 𝐯 = (𝑣𝑥 𝑣𝑦 1 𝜔𝑥 𝑣𝑧 1 𝜔𝑦 1 𝜔𝑧 1 𝜗̇1 𝑣𝑥 𝑣𝑦 2 𝜔𝑥 𝑣𝑧 2 𝜔𝑦 2 𝜔𝑧 2 𝜗̇2) , (8.62) where the superscript refers to the local node number. These are obtained by transforming the translational velocities and rotational velocities using the local to global transformation matrix qij. The strain rate – velocity matrix in the local system can be written 𝐁0 = −1 −𝑙0 ⎡ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎣ − −𝑙0 −1𝑧 −1 −1𝜔 𝑙0 −1𝑦 −𝑙0 𝑙0 −𝑙0 −1𝑧 𝑙0 −1 −𝑙0 −1 −𝑙0 ⎤ ⎥ ⎥ ⎥ ⎥ ⎥ ⎥ ⎥ 2 ⎦ where 𝑙0 is the beam length in the reference configuration, i.e., beginning of the time step. A corresponding matrix w.r.t. the current configuration is −1 −𝑙0 −1𝑦 𝑙0 −1𝑦 −1 𝑙0 −1 𝑙0 −1 𝑙0 −𝑙0 −1𝑧 −𝑙0 −1𝑦 𝑙0 −1𝑧 0 −1𝜔 𝑙0 − − − ,(8.63) LS-DYNA Theory Manual Warped Beam Elements 𝐁 = −𝑙−1 ⎡ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎣ −𝑙−1𝑧 −𝑙−1𝑦 −𝑙−1𝜔 𝑙−1 𝑙−1𝑧 −𝑙−1𝑦 𝑙−1𝜔 − 𝑙−1 𝑙−1𝑧 −𝑙−1 −𝑙−1 −𝑙−1𝑦 ⎤ ⎥ ⎥ ⎥ (8.64) , ⎥ ⎥ ⎥ ⎥ 2 ⎦ where we use the current length of the beam. These matrices are evaluated in each integration point (𝑥, 𝑦) of the cross section. To compute the strain rate in the local system we simply apply −𝑙−1𝑧 0 −𝑙−1 𝑙−1𝑦 𝑙−1 𝑙−1 − − − which is then used to update the local stresses 𝛔. The internal force vector is then assembled as 𝛆̇ = 𝐁0𝐯, (8.65) 𝐟 = 𝐁T𝛔. (8.66) Finally the internal force is transformed to the global system using the transformation matrix. To compute the stiffness matrix for implicit we neglect the geometric contribution and just apply where 𝐂 is the material tangent modulus. Again the matrix must be transformed to the global system before used in the implicit solver. 𝐊 = 𝐁T𝐂𝐁, (8.67) LS-DYNA Theory Manual Belytschko-Lin-Tsay Shell 9 Belytschko-Lin-Tsay Shell The Belytschko-Lin-Tsay shell element ([Belytschko and Tsay 1981], [Belytschko et al., 1984a]) was implemented in LS-DYNA as a computationally efficient alternative to the Hughes-Liu shell element. For a shell element with five through thickness integration points, the Belytschko-Lin-Tsay shell elements requires 725 mathematical operations compared to 4050 operations for the under integrated Hughes-Liu element. The selectively reduced integration formulation of the explicit Hughes-Liu element requires 35,350 mathematical operations. Because of its computational efficiency, the Belytschko-Lin-Tsay shell element is usually the shell element formulation of choice. For this reason, it has become the default shell element formulation for explicit calculations. The Belytschko-Lin-Tsay shell element is based on a combined co-rotational and velocity-strain formulation. The efficiency of the element is obtained from the mathematical simplifications that result from these two kinematical assumptions. The co-rotational portion of the formulation avoids the complexities of nonlinear mechanics by embedding a coordinate system in the element. The choice of velocity-strain or rate- of-deformation in the formulation facilitates the constitutive evaluation, since the conjugate stress is the physical Cauchy stress. We closely follow the notation of Belytschko, Lin, and Tsay in the following development. 9.1 Co-rotational Coordinates The midsurface of the quadrilateral shell element, or reference surface, is defined by the location of the element’s four corner nodes. An embedded element coordinate system that deforms with the element is defined in terms of these nodal coordinates. Then the procedure for constructing the co-rotational coordinate system begins by calculating a unit vector normal to the main diagonal of the element: Belytschko-Lin-Tsay Shell LS-DYNA Theory Manual y^ e^ r42 e^ s3 e^ r31 s1 x^ r21 Figure 9.1. Construction of element coordinate system is shown. 𝐞̂3 = 𝐬3 ∥𝐬3∥ , ∥𝐬3∥ = √[𝐬3]1 2 + [𝐬3]2 2, 2 + [𝐬3]3 𝐬3 = 𝐫31 × 𝐫42, (9.1) (9.2) (9.3) where the superscript caret (⋅ ̂) is used to indicate the local (element) coordinate system. It is desired to establish the local 𝑥 axis 𝑥̂ approximately along the element edge between nodes 1 and 2. This definition is convenient for interpreting the element stresses, which are defined in the local 𝑥̂ − 𝑦̂ coordinate system. The procedure for constructing this unit vector is to define a vector 𝐬1 that is nearly parallel to the vector 𝐫21, viz. 𝐬1 = 𝐫21 − (𝐫21 ⋅ 𝐞̂3)𝐞̂3, 𝐞̂1 = 𝐬1 ‖𝐬1‖ . The remaining unit vector is obtained from the vector cross product 𝐞̂2 = 𝐞̂3 × 𝐞̂1. (9.4) (9.5) (9.6) If the four nodes of the element are coplanar, then the unit vectors 𝐞̂1 and 𝐞̂2 are tangent to the midplane of the shell and 𝐞̂3 is in the fiber direction. As the element deforms, an angle may develop between the actual fiber direction and the unit normal 𝐞̂3. The magnitude of this angle may be characterized as 9-2 (Belytschko-Lin-Tsay Shell) ∣𝐞̂3 ⋅ 𝐟 − 1∣ < 𝛿, LS-DYNA Theory Manual Belytschko-Lin-Tsay Shell where 𝐟 is the unit vector in the fiber direction and the magnitude of 𝛿 depends on the magnitude of the strains. According to Belytschko et al., for most engineering applications, acceptable values of 𝛿 are on the order of 10-2 and if the condition presented in Equation (9.7) is met, then the difference between the rotation of the co- rotational coordinates 𝑒 ̂ and the material rotation should be small. The global components of this co-rotational triad define a transformation matrix between the global and local element coordinate systems. This transformation operates on vectors with global components 𝐀 = (𝐴𝑥 𝐴𝑦 𝐴𝑧) and element coordinate components 𝐀̂ = (𝐴̂𝑥 𝐴̂𝑦 𝐴̂𝑧), and is defined as: ⎧𝐴̂𝑥 ⎫ }} {{ 𝐴̂𝑦 ⎬ ⎨ }} {{ 𝐴̂𝑧⎭ ⎩ {⎧𝐴𝑥 }⎫ 𝐴𝑦 𝐴𝑧⎭}⎬ ⎩{⎨ = 𝛍𝐀̂ = 𝐪T𝐀̂, 𝑒3𝑥 ⎥⎤ 𝑒3𝑦 𝑒3𝑧⎦ 𝑒1𝑥 ⎢⎡ 𝑒1𝑦 𝑒1𝑧 ⎣ 𝑒2𝑥 𝑒2𝑦 𝑒2𝑧 𝐀 = = (9.8) where 𝑒𝑖𝑥, 𝑒𝑖𝑦, 𝑒𝑖𝑧 are the global components of the element coordinate unit vectors. The inverse transformation is defined by the matrix transpose, i.e., 𝐀̂ = 𝛍T𝐀. (9.9) 9.2 Velocity-Strain Displacement Relations The above small rotation condition, Equation (9.7), does not restrict the magnitude of the element’s rigid body rotations. Rather, the restriction is placed on the out-of-plane deformations, and, thus, on the element strain. Consistent with this restriction on the magnitude of the strains, the velocity-strain displacement relations used in the Belytschko-Lin-Tsay shell are also restricted to small strains. As in the Hughes-Liu shell element, the displacement of any point in the shell is partitioned into a midsurface displacement (nodal translations) and a displacement associated with rotations of the element’s fibers (nodal rotations). The Belytschko-Lin- Tsay shell element uses the Mindlin [1951] theory of plates and shells to partition the velocity of any point in the shell as: (9.10) where 𝐯 𝑚 is the velocity of the mid-surface, 𝛉 is the angular velocity vector, and 𝑧̂ is the distance along the fiber direction (thickness) of the shell element. The corresponding co-rotational components of the velocity strain (rate of deformation) are given by 𝐯 = 𝐯 𝑚 − 𝑧̂ 𝐞3 × 𝛉, 𝑑 ̂ 𝑖𝑗 = ( ∂𝜐̂𝑖 ∂𝑥̂𝑗 + ∂𝜐̂𝑗 ∂𝑥̂𝑖 ). (9.11) Substitution of Equation (9.10) into the above yields the following velocity-strain relations: Belytschko-Lin-Tsay Shell LS-DYNA Theory Manual 𝑑 ̂ 𝑥 = 𝑑 ̂ 𝑦 = ∂𝑣̂𝑥 ∂𝑥̂ ∂𝜐̂𝑦 ∂𝑦̂ + 𝑧̂ − 𝑧̂ ∂ 𝜃̂ ∂𝑥̂ , ∂ 𝜃̂ ∂𝑦̂ , 2𝑑 ̂ 𝑥𝑦 = ∂𝜐̂𝑥 ∂𝑦̂ + ∂𝜐̂𝑦 ∂𝑥̂ + 𝑧̂ ∂ 𝜃̂ ∂𝑦̂ ⎜⎛ ⎝ − ∂ 𝜃̂ ⎟⎞, ∂𝑥̂ ⎠ 2𝑑 ̂ 𝑦𝑧 = 2𝑑 ̂ 𝑥𝑧 = ∂𝜐̂𝑧 ∂𝑦̂ ∂𝜐̂𝑧 ∂𝑥̂ − 𝜃̂ 𝑥, + 𝜃̂ 𝑦. (9.12) (9.13) (9.14) (9.15) (9.16) The above velocity-strain relations need to be evaluated at the quadrature points within the shell. Standard bilinear nodal interpolation is used to define the mid-surface velocity, angular velocity, and the element’s coordinates (isoparametric representation). These interpolations relations are given by 𝐯𝑚 = 𝑁𝐼(𝜉 , 𝜂)𝐯𝐼, 𝛉𝑚 = 𝑁𝐼(𝜉 , 𝜂)𝛉𝐼, 𝐱𝑚 = 𝑁𝐼(𝜉 , 𝜂)𝐱𝐼. (9.17) where the subscript 𝐼 is summed over all the nodes of the element and the nodal velocities are obtained by differentiating the nodal coordinates with respect to time, i.e., 𝜐𝐼 = 𝑥̇𝐼. The bilinear shape functions are 𝑁1 = 𝑁2 = 𝑁3 = 𝑁4 = (1 − 𝜉 )(1 − 𝜂), (1 + 𝜉 )(1 − 𝜂), (1 + 𝜉 )(1 + 𝜂), (1 − 𝜉 )(1 + 𝜂). (9.18) (9.19) (9.20) (9.21) The velocity-strains at the center of the element, i.e., at 𝜉 = 0, and 𝜂 = 0, are obtained by substitution of the above relations into the previously defined velocity- strain displacement relations, Equations (9.12) and (9.16). After some algebra, this yields 𝑑 ̂ 𝑥 = 𝐵1𝐼𝜐̂𝑥𝐼 + 𝑧̂𝐵1𝐼𝜃̂ 𝑦𝐼, (9.22a) LS-DYNA Theory Manual Belytschko-Lin-Tsay Shell 𝑑 ̂ 𝑦 = 𝐵2𝐼𝜐̂𝑦𝐼 − 𝑧̂𝐵2𝐼𝜃̂ 𝑥𝐼, 2𝑑 ̂ 𝑥𝑦 = 𝐵2𝐼 𝜐̂𝑥𝐼 + 𝐵1𝐼𝜐̂𝑦𝐼 + 𝑧̂ (𝐵2𝐼𝜃̂ 𝑦𝐼 − 𝐵1𝐼𝜃̂ 𝑥𝐼), 2𝑑 ̂ 𝑥𝑧 = 𝐵1𝐼𝜐̂𝑧𝐼 + 𝑁𝐼𝜃̂ 𝑦𝐼, 2 𝑑 ̂ 𝑦𝑧 = 𝐵2𝐼 𝜐̂𝑧𝐼 − 𝑁𝐼 𝜃̂ 𝑥𝐼, 𝐵1𝐼 = 𝐵2𝐼 = ∂𝑁𝐼 ∂𝑥̂ , ∂𝑁𝐼 ∂𝑦̂ . (9.22b) (9.22c) (9.22d) (9.22e) (9.22f) (9.22g) The shape function derivatives 𝐵𝑎𝐼 are also evaluated at the center of the element, i.e., at 𝜉 = 0, and 𝜂 = 0. 9.3 Stress Resultants and Nodal Forces After suitable constitutive evaluations using the above velocity-strains, the resulting stresses are integrated through the thickness of the shell to obtain local resultant forces and moments. The integration formula for the resultants are 𝑓 ̂ 𝑅 = ∫ 𝜎̂𝛼𝛽𝑑𝑧̂, 𝛼𝛽 𝑚̂𝛼𝛽 𝑅 = − ∫ 𝑧̂𝜎̂𝛼𝛽𝑑𝑧̂, (9.23) (9.24) where the superscript, 𝑅, indicates a resultant force or moment, and the Greek subscripts emphasize the limited range of the indices for plane stress plasticity. The above element-centered force and moment resultants are related to the local nodal forces and moments by invoking the principle of virtual power and integrating with a one-point quadrature. The relations obtained in this manner are 𝑅 + 𝐵2𝐼𝑓 ̂ 𝑥𝐼 = 𝐴(𝐵1𝐼𝑓 ̂ 𝑓 ̂ 𝑅 ), 𝑥𝑦 𝑥𝑥 (9.25) 𝑅 + 𝐵1𝐼𝑓 ̂ 𝑦𝐼 = 𝐴(𝐵2𝐼𝑓 ̂ 𝑓 ̂ 𝑅 ), 𝑥𝑦 𝑦𝑦 𝑅 + 𝐵2𝐼𝑓 ̂ 𝑧𝐼 = 𝐴𝜅(𝐵1𝐼𝑓 ̂ 𝑓 ̂ 𝑅 ), 𝑦𝑧 𝑥𝑧 𝑚̂𝑥𝐼 = 𝐴 (𝐵2𝐼𝑚̂𝑦𝑦 𝑅 + 𝐵1𝐼𝑚̂𝑥𝑦 𝑅 − 𝑓 ̂ 𝑅 ), 𝑦𝑧 𝑚̂𝑦𝐼 = −𝐴 (𝐵1𝐼𝑚̂𝑥𝑥 𝑅 + 𝐵2𝐼𝑚̂𝑥𝑦 𝑅 − 𝑓 ̂ 𝑅 ), 𝑥𝑧 (9.26) (9.27) (9.28) (9.29) Belytschko-Lin-Tsay Shell LS-DYNA Theory Manual 𝑚̂𝑧𝐼 = 0, (9.30) where 𝐴 is the area of the element, and 𝜅 is the shear factor from the Mindlin theory. In the Belytschko-Lin-Tsay formulation, 𝜅 is used as a penalty parameter to enforce the Kirchhoff normality condition as the shell becomes thin. The above local nodal forces and moments are then transformed to the global coordinate system using the transformation relations given previously as Equation (9.8). The global nodal forces and moments are then appropriately summed over all the nodes and the global equations of motion are solved for the next increment in nodal accelerations. 9.4 Hourglass Control (Belytschko-Lin-Tsay) In part, the computational efficiency of the Belytschko-Lin-Tsay and the under integrated Hughes-Liu shell elements are derived from their use of one-point quadrature in the plane of the element. To suppress the hourglass deformation modes that accompany one-point quadrature, hourglass viscosity stresses are added to the physical stresses at the local element level. The discussion of the hourglass control that follows pertains to the Hughes-Liu and the membrane elements as well. The hourglass control used by Belytschko et al., extends an earlier derivation by Flanagan and Belytschko [1981], . The hourglass shape vector, 𝛕𝐼, is defined as 𝛕𝐼 = 𝐡𝐼 − (𝐡𝐽𝐱̂𝑎𝐽)𝐁𝑎𝐼, (9.31) where +1 ⎤ ⎡ −1 ⎥⎥ ⎢⎢ , +1 −1⎦ ⎣ is the basis vector that generates the deformation mode that is neglected by one-point quadrature. In Equation (9.31) and the reminder of this subsection, the Greek subscripts have a range of 2, e.g., 𝐱̂𝑎𝐼 = (𝑥̂1𝐼, 𝑥̂2𝐼) = (𝑥̂𝐼, 𝑦̂𝐼). 𝐡 = (9.32) The hourglass shape vector then operates on the generalized displacements, in a manner similar to Equations (7.11a - e), to produce the generalized hourglass strain rates 𝐵 = 𝛕𝐼𝜃̂ 𝐪̇𝛼 𝛼𝐼, 𝐵 = 𝝉𝐼𝜐̂𝑧𝐼, 𝐪̇3 (9.33) (9.34) LS-DYNA Theory Manual Belytschko-Lin-Tsay Shell where the superscripts 𝐁 and 𝐌 denote bending and membrane modes, respectively. The corresponding hourglass stress rates are then given by 𝑀 = 𝛕𝐼𝜐̂𝛼𝐼, 𝐪̇𝛼 (9.35) 𝑄̇𝛼 𝐵 = 𝑟𝜃𝐸𝑡3𝐴 192 𝐵, 𝐵𝛽𝐼𝐵𝛽𝐼𝑞 ̇𝛼 𝑄̇3 𝐵 = 𝑟𝑤𝜅𝐺𝑡3𝐴 12 𝐵, 𝐵𝛽𝐼𝐵𝛽𝐼𝑞 ̇3 𝑄̇𝛼 𝑀 = 𝑟𝑚𝐸𝑡𝐴 𝐵𝛽𝐼𝐵𝛽𝐼𝑞 ̇𝛼 𝑀, (9.36) (9.37) (9.38) where 𝑡 is the shell thickness and the parameters, 𝑟𝜃, 𝑟𝑤, and 𝑟𝑚 are generally assigned values between 0.01 and 0.05. Finally, the hourglass stresses, which are updated from the stress rates in the usual way, i.e., and the hourglass resultant forces are then 𝐐𝑛+1 = 𝐐𝑛 + Δ𝑡𝐐̇ , 𝑚̂𝛼𝐼 𝐵, 𝐻 = 𝜏𝐼𝑄𝛼 𝐵, 𝑓 ̂ 𝐻 = 𝜏𝐼𝑄3 3𝐼 𝑓 ̂ 𝑀, 𝐻 = 𝜏𝐼𝑄𝛼 𝛼𝐼 (9.39) (9.40) (9.41) (9.42) where the superscript 𝐻 emphasizes that these are internal force contributions from the hourglass deformations. These hourglass forces are added directly to the previously determined local internal forces due to deformations Equations (7.14a - f). These force vectors are orthogonalized with respect to rigid body motion. 9.5 Hourglass Control (Englemann and Whirley) Englemann and Whirley [1991] developed an alternative hourglass control, which they implemented in the framework of the Belytschko, Lin, and Tsay shell element. We will briefly highlight their procedure here that has proven to be cost effective-only twenty percent more expensive than the default control. In the hourglass procedure, the in-plane strain field (subscript p) is decomposed into the one point strain field plus the stabilization strain field: 𝑠 , 0 + 𝛆̅ ̇p ̇p ̇p = 𝛆̅ 𝛆̅ (9.43) Belytschko-Lin-Tsay Shell LS-DYNA Theory Manual 𝑠 = 𝐖𝑚𝐪̇𝑚 + 𝑧𝐖𝑏𝐪̇𝑏. ̇p 𝛆̅ (9.44) Here, 𝐖𝑚 and 𝐖𝑏 play the role of stabilization strain velocity operators for membrane and bending: 𝐖𝑚 = 𝑝(𝜉 , 𝜂) 𝑓1 ⎡ 𝑝(𝜉 , 𝜂) ⎢ 𝑓2 ⎢ 𝑝(𝜉 , 𝜂) 𝑓3 ⎣ 𝑝(𝜉 , 𝜂) 𝑓4 ⎤ 𝑝(𝜉 , 𝜂) ⎥ , 𝑓5 ⎥ 𝑝(𝜉 , 𝜂)⎦ 𝑓6 𝐖𝑏 = −𝑓4 ⎡ ⎢ −𝑓5 ⎢ −𝑓6 ⎣ 𝑝(𝜉 , 𝜂) 𝑝(𝜉 , 𝜂) 𝑝(𝜉 , 𝜂) 𝑝(𝜉 , 𝜂) 𝑓1 ⎤ 𝑝(𝜉 , 𝜂) ⎥ , 𝑓2 ⎥ 𝑝(𝜉 , 𝜂)⎦ 𝑓3 (9.45) (9.46) where the terms 𝑓𝑖 to the reference [Englemann and Whirley, 1991]. 𝑝(𝜉 , 𝜂) 𝑖 = 1, 2, . . . , 6, are rather complicated and the reader is referred To obtain the transverse shear assumed strain field, the procedure given in [Bathe and Dvorkin, 1984] is used. The transverse shear strain field can again be decomposed into the one point strain field plus the stabilization field: that is related to the hourglass velocities by 𝑠, 0 + 𝛆̅ ̇s ̇s ̇s = 𝛆̅ 𝛆̅ 𝑠 = 𝐖s𝐪̇𝑠, ̇s 𝛆̅ where the transverse shear stabilization strain-velocity operator 𝐖𝑠 is given by 𝑠(𝜉 , 𝜂) −𝑔1 𝑠𝜉 𝑓1 𝑠𝜉 𝑠(𝜉 , 𝜂) 𝑔4 𝑓2 𝑠(𝜉 , 𝜂) and 𝑔1 𝑠𝜉 𝑠𝜂 𝑔2 𝑔3 𝑠𝜉 𝑠𝜂 −𝑔2 𝑔4 𝑠 are defined in the reference. Again, the coefficients 𝑓1 𝑠𝜂 𝑔3 𝑠𝜂 𝑔1 𝐖𝑠 = [ ]. (9.47) (9.48) (9.49) In their formulation, the hourglass forces are related to the hourglass velocity field through an incremental hourglass constitutive equation derived from an additive decomposition of the stress into a “one-point stress,” plus a “stabilization stress.” The integration of the stabilization stress gives a resultant constitutive equation relating hourglass forces to hourglass velocities. The in-plane and transverse stabilization stresses are updated according to: 𝑠,𝑛+1 = 𝛕s 𝛕s 𝑠, 𝑠,𝑛 + Δ𝑡𝑐𝑠𝐂𝑠𝛆̅ ̇𝑠 (9.50) 𝑠, 𝑠,𝑛 + Δ𝑡𝑐s𝐂s𝛆̅ ̇s where the tangent matrix is the product of a matrix 𝐂, which is constant within the shell domain, and a scalar 𝑐 that is constant in the plane but may vary through the thickness. 𝑠,𝑛+1 = 𝛕s 𝛕s (9.51) The stabilization stresses can now be used to obtain the hourglass forces: LS-DYNA Theory Manual Belytschko-Lin-Tsay Shell Figure 9.2. The twisted beam problem fails with the Belytschko-Tsay shell element. 𝐐𝑚 = ∫ ∫ 𝐖𝑚 −ℎ T 𝛕𝑝 𝑠 𝑑𝐴 , 𝑑𝑧 𝐐𝑏 = ∫ ∫ 𝐖𝑏 −ℎ T𝛕𝑝 𝑠 𝑑𝐴 𝐐𝑠 = ∫ ∫ 𝐖𝑠 −ℎ T𝛕𝑠 𝑠𝑑𝐴 𝑑𝑧 , 𝑑𝑧 . (9.52) (9.53) (9.54) 9.6 Belytschko-Wong-Chiang Improvements Since the Belytschko-Tsay element is based on a perfectly flat geometry, warpage is not considered. Although this generally poses no major difficulties and provides for an efficient element, incorrect results in the twisted beam problem, See Figure 7.2, are obtained where the nodal points of the elements used in the discretization are not coplanar. The Hughes-Liu shell element considers non-planar geometry and gives good results on the twisted beam, but is relatively expensive. The effect of neglecting warpage in typical a application cannot be predicted beforehand and may lead to less than accurate results, but the latter is only speculation and is difficult to verify in practice. Obviously, it would be better to use shells that consider warpage if the added costs are reasonable and if this unknown effect is eliminated. In this section we briefly describe the simple and computationally inexpensive modifications necessary in the Belytschko-Tsay shell to include the warping stiffness. The improved transverse shear treatment is also described which is necessary for the element to pass the Kirchhoff Belytschko-Lin-Tsay Shell LS-DYNA Theory Manual P3 P1 P2 Figure 9.3. Nodal fiber vectors 𝐩1, 𝐩2, and 𝐩3, where ℎ is the thickness. patch test. Readers are directed to the references [Belytschko, Wong, and Chang 1989, 1992] for an in depth theoretical background. In order to include warpage in the formulation it is convenient to define nodal fiber vectors as shown in Figure 7.3. The geometry is interpolated over the surface of the shell from: where 𝑥 = 𝑥𝑚 + 𝜁 ̅𝑝 = (𝑥𝐼 + 𝜁 ̅𝑝𝐼)𝑁𝐼(𝜉 , 𝜂), 𝜁 ̅ = 𝜁ℎ . The in plane strain components are given by: 𝑑𝑥𝑥 = 𝑏𝑥𝐼𝑣̂𝑥𝐼 + 𝜁 ̅(𝑏𝑥𝐼 𝑐 𝑣̂𝑥𝐼 + 𝑏𝑥𝐼𝑝̇𝑥𝐼), 𝑑𝑦𝑦 = 𝑏𝑦𝐼𝑣̂𝑦𝐼 + 𝜁 ̅(𝑏𝑦𝐼 𝑐 𝑣̂𝑦𝐼 + 𝑏𝑦𝐼𝑝̇𝑦𝐼), 𝑑𝑥𝑦 = 𝑏𝑥𝐼𝑣̂𝑦𝐼 + 𝑏𝑦𝐼𝑣̂𝑥𝐼 + 𝜁 ̅(𝑏𝑥𝐼 𝑐 𝑣̂𝑦𝐼 + 𝑏𝑥𝐼𝑝̇𝑦𝐼 + 𝑏𝑦𝐼 𝑐 𝑣̂𝑥𝐼 + 𝑏𝑦𝐼𝑝̇𝑥𝐼). (9.55) (9.56) (9.57) (9.58) (9.59) The coupling terms are come in through 𝑏𝑖𝐼 components of the fiber vectors as: 𝑐 : which is defined in terms of the 𝑏𝑥𝐼 𝑐 } = [ 𝑏𝑦𝐼 { 𝑝𝑦̂2 − 𝑝𝑦̂4 𝑝𝑥̂2 − 𝑝𝑥̂4 𝑝𝑦̂3 − 𝑝𝑦̂1 𝑝𝑥̂3 − 𝑝𝑥̂1 𝑝𝑦̂4 − 𝑝𝑦̂2 𝑝𝑥̂4 − 𝑝𝑥̂2 𝑝𝑦̂1 − 𝑝𝑦̂3 𝑝𝑥̂1 − 𝑝𝑥̂3 ], (9.60) For a flat geometry the normal vectors are identical and no coupling can occur. 𝑐 and the reader is referred to his Two methods are used by Belytschko for computing 𝑏𝑖𝐼 papers for the details. Both methods have been tested in LS-DYNA and comparable results were obtained. The transverse shear strain components are given as LS-DYNA Theory Manual Belytschko-Lin-Tsay Shell y^ ey^ Lk enk eni ex^ Figure 9.4. Vector and edge definitions for computing the transverse shear strain components. 𝛾̂𝑥𝑧 = −𝑁𝐼(𝜉 , 𝜂)𝜃̅ 𝑦̂𝐼, 𝛾̂𝑦𝑧 = −𝑁𝐼(𝜉 , 𝜂)𝜃̅ 𝑥̂𝐼, where the nodal rotational components are defined as: 𝐾, 𝐾 ⋅ 𝐞𝑥̂)𝜃̅ 𝐼 + (𝐞𝑛 𝐼 ⋅ 𝐞𝑥̂)𝜃̅ 𝜃̅ 𝑥̂𝐼 = (𝐞𝑛 𝜃̅ 𝑦̂𝐼 = (𝐞𝑛 𝐼 + (𝐞𝑛 𝐼 ⋅ 𝐞𝑦̂)𝜃̅ 𝐾, 𝐾 ⋅ 𝐞𝑦̂)𝜃̅ 𝐼 = 𝜃̅ (𝜃𝑛𝐼 𝐼 + 𝜃𝑛𝐽 𝐼 ) + 𝐿𝐼𝐽 (𝜐̂𝑧𝐽 − 𝜐̂𝑧𝐽), (9.61) (9.62) (9.63) (9.64) (9.65) where the subscript n refers to the normal component of side 𝐼 as seen in Figure 7.3 and 𝐿𝐼𝐽 is the length of side 𝐼𝐽. LS-DYNA Theory Manual Triangular Shells 10 Triangular Shells 10.1 C0 Triangular Shell The 𝐶0 shell element due to Kennedy, Belytschko, and Lin [1986] has been implemented as a computationally efficient triangular element complement to the Belytschko-Lin-Tsay quadrilateral shell element ([Belytschko and Tsay 1981], [Belytschko et al., 1984a]). For a shell element with five through-the-thickness integration points, the element requires 649 mathematical operations (the Belytschko- Lin-Tsay quadrilateral shell element requires 725 mathematical operations) compared to 1417 operations for the Marchertas-Belytschko triangular shell [Marchertas and Belytschko 1974] (referred to as the BCIZ [Bazeley, Cheung, Irons, and Zienkiewicz 1965] triangular shell element in the DYNA3D user’s manual). Triangular shell elements are offered as optional elements primarily for compatibility with local user grid generation and refinement software. Many computer aided design (CAD) and computer aided manufacturing (CAM) packages include finite element mesh generators, and most of these mesh generators use triangular elements in the discretization. Similarly, automatic mesh refinement algorithms are typically based on triangular element discretization. Also, triangular shell element formulations are not subject to zero energy modes inherent in quadrilateral element formulations. The triangular shell element’s origins are based on the work of Belytschko et al., [Belytschko, Stolarski, and Carpenter 1984b] where the linear performance of the shell was demonstrated. Because the triangular shell element formulations parallels closely the formulation of the Belytschko-Lin-Tsay quadrilateral shell element presented in the previous section (Section 7), the following discussion is limited to items related specifically to the triangular shell element. 10.1.1 Co-rotational Coordinates The mid-surface of the triangular shell element, or reference surface, is defined by the location of the element’s three nodes. An embedded element coordinate system Triangular Shells LS-DYNA Theory Manual y^ z^ e^ e^ e^ x^ Figure 10.1. Local element coordinate system for C0 shell element. that deforms with the element is defined in terms of these nodal coordinates. The procedure for constructing the co-rotational coordinate system is simpler than the corresponding procedure for the quadrilateral, because the three nodes of the triangular element are guaranteed coplanar. The local x-axis 𝑥̂ is directed from node 1 to 2. The element’s normal axis 𝑧̂ is defined by the vector cross product of a vector along 𝑥̂ with a vector constructed from node 1 to node 3. The local y-axis 𝑦̂ is defined by a unit vector cross product of 𝐞̂3 with 𝐞̂1, which are the unit vectors in the 𝑧̂ directions, respectively. As in the case of the quadrilateral element, this triad of co-rotational unit vectors defines a transformation between the global and local element coordinate systems. See Equations (7.5 a, b). 10.1.2 Velocity-Strain Relations As in the Belytschko-Lin-Tsay quadrilateral shell element, the displacement of any point in the shell is partitioned into a mid-surface displacement (nodal translations) and a displacement associated with rotations of the element’s fibers (nodal rotations). The Kennedy-Belytschko-Lin triangular shell element also uses the Mindlin [Mindlin 1951] theory of plates and shells to partition the velocity of any point in the shell (recall Equation (7.6)): 𝐯 = 𝐯m − 𝑧̂ 𝐞3 × 𝛉, (10.1) where 𝐯m is the velocity of the mid-surface, 𝛉 is the angular velocity vector, and 𝑧̂ is the distance along the fiber direction (thickness) of the shell element. The corresponding co-rotational components of the velocity strain (rate of deformation) were given previously in Equation (7.11 a - e). Standard linear nodal interpolation is used to define the midsurface velocity, angular velocity, and the element’s coordinates (isoparametric representation). These interpolation triangular element formulations. Substitution of the nodally interpolated velocity fields into the velocity- strain relations , leads to strain rate-velocity relations of the form the area coordinates used functions are in 10-2 (Triangular Shells) 𝐝̂ = 𝐁 𝐯̂. LS-DYNA Theory Manual Triangular Shells It is convenient to partition the velocity strains and the 𝐁 matrix into membrane and bending contributions. The membrane relations are given by ⎧ 𝑑 ̂ {{ 𝑑 ̂ ⎨ {{ 2𝑑 ̂ ⎩ ⎫ }} ⎬ }} 𝑥𝑦⎭ = 𝑦̂3 ⎡ ⎢ 𝑥̂2𝑦̂3 ⎣ 𝑥̂3 − 𝑥̂2 𝑥̂3 − 𝑥̂2 −𝑦̂3 𝑦̂3 −𝑥̂3 −𝑥̂3 𝑦̂3 𝑥̂2 ⎤ 𝑥̂2 ⎥ 0 ⎦ ⎫ ⎧𝜐̂𝑥1 𝜐̂𝑦1 𝜐̂𝑥2 𝜐̂𝑦2 𝜐̂𝑥3 𝜐̂𝑦3⎭ {{{{{ {{{{{ }}}}} }}}}} ⎬ ⎨ ⎩ , (10.3) 𝐝̂M = 𝐁M 𝐯̂, (10.4) ⎧ 𝜅̂𝑥 ⎫ } { 𝜅̂𝑦 ⎬ ⎨ } { 2𝜅̂𝑥𝑦⎭ ⎩ = −1 ⎡ 𝑥̂3 − 𝑥̂2 ⎢ 𝑥̂2𝑦̂3 ⎣ 𝑦̂3 or −𝑦̂3 𝑦̂3 𝑥̂3 − 𝑥̂2 −𝑦̂3 −𝑥̂3 𝑥̂3 −𝑥̂2 ⎤ ⎥ 𝑥̂2⎦ ⎫ ⎧𝜃̂ 𝑥1 𝜃̂ 𝑦1 𝜃̂ 𝑥2 ⎨ 𝜃̂ 𝑦2 𝜃̂ 𝑥3 𝜃̂ 𝑦3⎭ ⎩ {{{{{{ {{{{{{ }}}}}} }}}}}} ⎬ , (10.5) 𝛋̂M = 𝐁M𝛉̂ def. (10.6) The local element velocity strains are then obtained by combining the above two relations: ⎧ 𝑑 ̂ {{ 𝑑 ̂ ⎨ {{ 2𝑑 ̂ ⎩ ⎫ }} ⎬ }} 𝑥𝑦⎭ = ⎧ 𝑑 ̂ {{ 𝑑 ̂ ⎨ {{ 2𝑑 ̂ ⎩ ⎫ }} ⎬ }} 𝑥𝑦⎭ − 𝑧̂ ⎧ 𝜅̂𝑥 ⎫ } { 𝜅̂𝑦 ⎬ ⎨ } { 2𝜅̂𝑥𝑦⎭ ⎩ = 𝐝̂M − 𝑧̂𝛋̂. (10.7) The remaining two transverse shear strain rates are given by { 6 𝑥̂2 𝑦̂3 } = 2𝑑 ̂ 𝑥𝑧 2𝑑 ̂ 𝑦𝑧 −𝑦̂3 [ 𝑦̂3( 𝑥̂2 − 2𝑥̂2) 𝑦̂3 (2 𝑥̂2 + 𝑥̂3) 𝑦̂3 2 − 𝑥̂3 𝑥̂2 −𝑦̂3 𝑦̂3(3 𝑥̂2 − 𝑥̂3) 2( 𝑥̂2 + 𝑥̂3) 𝑥̂3( 𝑥̂3 − 2𝑥̂2) −3𝑥̂2𝑦̂3 (10.8) 𝑥̂2𝑦̂3 ] 𝑥̂2( 2𝑥̂3 − 𝑥̂2) Triangular Shells LS-DYNA Theory Manual def , ⎫ ⎧𝜃̂ 𝑥1 𝜃̂ 𝑦1 𝜃̂ 𝑥2 𝜃̂ 𝑦2 𝜃̂ 𝑥3 𝜃̂ 𝑦3⎭ {{{{{{ {{{{{{ }}}}}} }}}}}} ⎨ ⎩ ⎬ All of the above velocity-strain relations have been simplified by using one-point quadrature. 𝐝̂S = 𝐁S𝛉̂ def. (10.9) In the above relations, the angular velocities 𝛉̂def are the deformation component of the angular velocity 𝛉̂ obtained by subtracting the portion of the angular velocity due to rigid body rotation, i.e., The two components of the rigid body angular velocity are given by 𝛉̂def = 𝛉̂ − 𝛉̂rig, rig = 𝜃̂ 𝜐̂𝑧1 − 𝜐̂𝑧2 𝑥̂2 , (10.10) (10.11) rig = 𝜃̂ (𝜐̂𝑧3 − 𝜐̂𝑧1)𝑥̂2 − (𝜐̂𝑧2 − 𝜐̂𝑧1)𝑥̂3 𝑥̂2𝑦̂3 The first of the above two relations is obtained by considering the angular velocity of the local x-axis about the local y-axis. Referring to Figure 10.1, by construction nodes 1 and 2 lie on the local x-axis and the distance between the nodes is 𝑥̂2 i.e., the 𝑥̂ distance from node 2 to the local coordinate origin at node 1. Thus the difference in the nodal 𝑧̂ velocities divided by the distance between the nodes is an average measure of the rigid body rotation rate about the local y-axis. (10.12) . The second relation is conceptually identical, but is implemented in a slightly different manner due to the arbitrary location of node 3 in the local coordinate system. Consider the two local element configurations shown in Figure 10.2. For the leftmost configuration, where node 3 is the local y-axis, the rigid body rotation rate about the local x-axis is given by rig = 𝜃̂ 𝑥−left 𝜐̂𝑧3 − 𝜐̂𝑧1 𝑦̂3 , and for the rightmost configuration the same rotation rate is given by rig 𝜃̂ 𝑥−right = 𝜐̂𝑧3 − 𝜐̂𝑧2 𝑦̂3 . (10.13) (10.14) LS-DYNA Theory Manual Triangular Shells z^ y^ z^ x^ y^ x^ Figure 10.2. Element configurations with node 3 aligned with node 1 (left) and node 3 aligned with node 2 (right). Although both of these relations yield the average rigid body rotation rate, the selection of the correct relation depends on the configuration of the element, i.e., on the location of node 3. Since every element in the mesh could have a configuration that is different in general from either of the two configurations shown in Figure 10.2, a more robust relation is needed to determine the average rigid body rotation rate about the local x- axis. In most typical grids, node 3 will be located somewhere between the two configurations shown in Figure 10.2. Thus a linear interpolation between these two rigid body rotation rates was devised using the distance 𝑥̂3 as the interpolant: rig = 𝜃̂ 𝜃̂ rig (1 − 𝑥−left 𝑥̂3 𝑥̂2 ) + 𝜃̂ rig 𝑥−right ( 𝑥̂3 𝑥̂2 ). (10.15) Substitution of Equations (10.13) and (10.14) into (10.15) and simplifying produces the relations given previously as Equation (10.12). Triangular Shells LS-DYNA Theory Manual 10.1.3 Stress Resultants and Nodal Forces After suitable constitutive evaluation using the above velocity strains, the resulting local stresses are integrated through the thickness of the shell to obtain local resultant forces and moments. The integration formulae for the resultants are 𝑓 ̂ 𝑅 = ∫ 𝜎̂𝛼𝛽𝑑𝑧̂, 𝛼𝛽 𝑚̂𝛼𝛽 𝑅 = − ∫ 𝑧̂ 𝜎̂𝛼𝛽𝑑𝑧̂, (10.16) (10.17) where the superscript 𝑅 indicates a resultant force or moment and the Greek subscripts emphasize the limited range of the indices for plane stress plasticity. The above element-centered force and moment resultant are related to the local nodal forces and moments by invoking the principle of virtual power and performing a one-point quadrature. The relations obtained in this manner are ⎧𝑓 ̂ ⎫ 𝑥1 } { } { 𝑓 ̂ } { 𝑦1 } { } { 𝑓 ̂ } { 𝑥2 ⎬ ⎨ 𝑓 ̂ } { 𝑦2 } { } { 𝑓 ̂ } { 𝑥3 } { } { 𝑓 ̂ ⎩ 𝑦3⎭ = 𝐴𝐁M ⎧𝑓 ̂ 𝑥𝑥 {{ 𝑓 ̂ ⎨ 𝑦𝑦 {{ 𝑓 ̂ ⎩ 𝑥𝑦 ⎫ }} ⎬ }} ⎭ , = 𝐴𝐁M ⎧𝑚̂𝑥𝑥 {{ 𝑚̂𝑦𝑦 ⎨ {{ 𝑚̂𝑥𝑦 ⎩ ⎫ }} ⎬ }} ⎭ + 𝐴𝐁S T { 𝑓 ̂ 𝑅 𝑥𝑧 𝑅}, 𝑓 ̂ 𝑦𝑧 (10.18) (10.19) ⎫ ⎧𝑚̂𝑥1 𝑚̂𝑦1 𝑚̂𝑥2 𝑚̂𝑦2 𝑚̂𝑥3 𝑚̂𝑦3⎭ {{{{{ {{{{{ }}}}} }}}}} ⎬ ⎨ ⎩ where 𝐴 is the area of the element (2𝐴 = 𝑥̂2𝑦̂3). The remaining nodal forces, the 𝑧̂ component of the force (𝑓 ̂ determined by successively solving the following equilibration equations 𝑚̂𝑥1 + 𝑚̂𝑥2 + 𝑚̂𝑥3 + 𝑦̂3𝑓 ̂ 𝑧3 = 0, 𝑧3 , 𝑓 ̂ 𝑧2 , 𝑓 ̂ 𝑧1), are 𝑚̂𝑦1 + 𝑚̂𝑦2 + 𝑚̂𝑦3 − 𝑥̂3𝑓 ̂ 𝑧3 − 𝑥̂2𝑓 ̂ 𝑧2 = 0, 𝑧1 + 𝑓 ̂ 𝑓 ̂ 𝑧2 + 𝑓 ̂ 𝑧3 = 0, (10.20) (10.21) (10.22) which represent moment equilibrium about the local x-axis, moment equilibrium about the local y-axis, and force equilibrium in the local z-direction, respectively. LS-DYNA Theory Manual Triangular Shells 10.2 Marchertas-Belytschko Triangular Shell The Marchertas-Belytschko [1974] triangular shell element, or the BCIZ triangular shell element as it is referred to in the LS-DYNA user’s manual, was developed in the same time period as the Belytschko beam element [Belytschko, Schwer, and Klein, 1977], see Section 4, forming the first generation of co-rotational structural elements developed by Belytschko and co-workers. This triangular shell element became the first triangular shell implemented in DYNA3D. Although the Marchertas-Belytschko shell element is relatively expensive, i.e., the 𝐶0 triangular shell element with five through-the-thickness integration points requires 649 mathematical operations compared to 1,417 operations for the Marchertas-Belytschko triangular shell, it is maintained in LS-DYNA for compatibility with earlier user models. However, as the LS-DYNA user community moves to application of the more efficient shell element formulations, the use of the Marchertas-Belytschko triangular shell element will decrease. As mentioned above, the Marchertas-Belytschko triangular shell has a common co-rotational formulation origin with the Belytschko beam element. The interested reader is referred to the beam element description, see Section 4, for details on the co- rotational formulation. In the next subsection a discussion of how the local element coordinate system is identical for the triangular shell and beam elements. The remaining subsections discuss the triangular element’s displacement interpolants, the strain displacement relations, and calculations of the element nodal forces. In the report [1974], much greater detail is provided. 10.2.1 Element Coordinates Figure 10.3(a) shows the element coordinate system, (𝐱̂, 𝐲̂, 𝐳̂) originating at Node 1, for the Marchertas-Belytschko triangular shell. The element coordinate system is associated with a triad of unit vectors (𝐞1, 𝐞2, 𝐞3) the components of which form a transformation matrix between the global and local coordinate systems for vector quantities. The nodal or body coordinate system unit vectors (𝐛1, 𝐛2, 𝐛3) are defined at each node and are used to define the rotational deformations in the element, see Section 8.4.4. The unit normal to the shell element 𝐞3 is formed from the vector cross product 𝐞3 = 𝐥21 × 𝐥31, (10.23) where 𝐥21 and 𝐥31 are unit vectors originating at Node 1 and pointing towards Nodes 2 and 3 respectively, see Figure 10.3(b). Next a unit vector g, see Figure 10.3(b), is assumed to be in the plane of the triangular element with its origin at Node 1 and forming an angle 𝛽 with the element side between Nodes 1 and 2, i.e., the vector 𝑙21. The direction cosines of this unit vector Triangular Shells LS-DYNA Theory Manual are represented by the symbols (𝑔𝑥, 𝑔𝑦, 𝑔𝑧). Since g is the unit vector, its direction cosines will satisfy the equation 𝑔𝑥 2 + 𝑔𝑦 2 + 𝑔𝑧 2 = 1. (10.24) Also, since 𝐠 and 𝐞3 are orthogonal unit vectors, their vector dot product must satisfy the equation 𝑒3𝑥𝑔𝑥 + 𝑒3𝑦𝑔𝑦 + 𝑒3𝑧𝑔𝑧 = 0. (10.25) In addition, the vector dot product of the co-planar unit vectors 𝐠 and 𝐥21 satisfies the equation 𝐼21𝑥𝑔𝑥 + 𝐼21𝑦𝑔𝑦𝑔𝑦 + 𝐼21𝑧𝑔𝑧 = cos𝛽, (10.26) where (𝑙21𝑥, 𝑙21𝑦, 𝑙21𝑧)are the direction cosines of 𝐥21. LS-DYNA Theory Manual Triangular Shells y^ z^ e2 e3 e1 x^ b2 (a) Element and body coordinates b3 b1 y^ z^ e2 I31 e3 α/2 I21 x^ b2 b3 b1 (b) Construction of element coordinates Figure 10.3. Construction of local element coordinate system. Solving this system of three simultaneous equation, i.e., Equation (10.24), (10.25), and (10.26), for the direction cosines of the unit vector g yields 𝑔𝑥 = 𝑙21𝑥cos𝛽 + (𝑒3𝑦𝑙21𝑧 − 𝑒3𝑧𝑙21𝑦)sin𝛽, 𝑔𝑦 = 𝑙21𝑦cos𝛽 + (𝑒3𝑧𝑙21𝑥 − 𝑒3𝑥𝑙21𝑧)sin𝛽, (10.27) (10.28) Triangular Shells LS-DYNA Theory Manual 𝑔𝑧 = 𝑙21𝑧cos𝛽 + (𝑒3𝑥𝑙21𝑦 − 𝑒3𝑦𝑙21𝑥)sin𝛽. (10.29) These equations provide the direction cosines for any vector in the plane of the triangular element that is oriented at an angle 𝛽 from the element side between Nodes 1 and 2. Thus the unit vector components of 𝐞1 and 𝐞2 are obtained by setting 𝛽 = 𝛼/2 and 𝛽 = (𝜋 + 𝛼)/2 in Equation (8.22), respectively. The angle 𝛼 is obtained from the vector dot product of the unit vectors 𝐥21 and 𝐥31, cos𝛼 = 𝐥21 ⋅ 𝐥31. (10.30) 10.2.2 Displacement Interpolation As with the other large displacement and small deformation co-rotational element formulations, the nodal displacements are separated into rigid body and deformation displacements, 𝐮 = 𝐮rigid + 𝐮def, (10.31) where the rigid body displacements are defined by the motion of the local element coordinate system, i.e., the co-rotational coordinates, and the deformation displacement are defined with respect to the co-rotational coordinates. The deformation displacement are defined by def ⎧ 𝑢̂𝑥 {{ 𝑢̂𝑦 ⎨ − − − {{ ⎩ ⎫ }} ⎬ }} 𝑢̂𝑧 ⎭ = 𝜙𝑥 𝜙𝑦 − − − 𝜙𝑧 ⎡ ⎢ ⎢ ⎢ ⎣ ⎤ ⎥ ⎥ ⎥ ⎦ {⎧ 𝛿 }⎫ − − − 𝜃̂ ⎭}⎬ ⎩{⎨ , 𝛅T = {𝛿12 𝛿23 𝛿31}, are the edge elongations and 𝛉̂ = {𝜃̂ 1𝑥 𝜃̂ 1𝑦 𝜃̂ 2𝑥 𝜃̂ 2𝑦 𝜃̂ 3𝑥 𝜃̂ 3𝑦}, are the local nodal rotation with respect to the co-rotational coordinates. (10.32) (10.33) (10.34) 𝑚, 𝜙𝑦 𝑚 and 𝜙𝑧 The matrices 𝜙𝑥 𝑓 are the membrane and flexural interpolation functions, respectively. The element’s membrane deformation is defined in terms of the edge elongations. Marchertas and Belytschko adapted this idea from Argyris et al., [1964], where incremental displacements are used, by modifying the relations for total displacements, 𝛿𝑖𝑗 = 2(𝑥𝑗𝑖𝑢𝑗𝑖𝑥 + 𝑦𝑗𝑖𝑢𝑗𝑖𝑦 + 𝑧𝑗𝑖𝑢𝑗𝑖𝑧) + 𝑢𝑗𝑖𝑥 2 + 𝑢𝑗𝑖𝑦 2 + 𝑢𝑗𝑖𝑧 0 + 𝑙𝑖𝑗 𝑙 𝑖𝑗 , (10.35) where 𝑥𝑗𝑖 = 𝑥𝑗 − 𝑥𝑖, etc. The non-conforming shape functions used for interpolating the flexural 𝑓 were originally derived by Bazeley, Cheung, Irons, and Zienkiewicz deformations, 𝜙𝑧 LS-DYNA Theory Manual Triangular Shells 𝑓 [1965]; hence the LS-DYNA reference to the BCIZ element. Explicit expressions for 𝜙𝑧 are quite tedious and are not given here. The interested reader is referred to Appendix G in the original work of Marchertas and Belytschko [1974]. The local nodal rotations, which are interpolated by these flexural shape functions, are defined in a manner similar to those used in the Belytschko beam element. The current components of the original element normal are obtained from the relation 0, 0 = 𝛍T𝛌𝐞̅ 3 𝐞3 (10.36) where 𝛍 and 𝛌 are the current transformations between the global coordinate system 0 is the and the element (local) and body coordinate system, respectively. The vector 𝐞̅ 3 original element unit normal expressed in the body coordinate system. The vector cross product between this current-original unit normal and the current unit normal, 𝐞3 × 𝐞3 0 = 𝜃̂ 𝑥𝐞1 + 𝜃̂ 𝑦𝐞2, define the local nodal rotations as 0 , 𝛉̂𝑥 = − 𝐞̂3𝑦 0 . 𝛉̂𝑦 = 𝐞̂3𝑥 (10.37) (10.38) (10.39) Note that at each node the corresponding 𝛌 transformation matrix is used in Equation (10.36). 10.2.3 Strain-Displacement Relations Marchertas-Belytschko impose the usual Kirchhoff assumptions that normals to the midplane of the element remain straight and normal, to obtain 𝑒𝑥𝑥 = 𝑒𝑦𝑦 = ∂𝑢𝑥 ∂𝑥 ∂𝑢𝑦 ∂𝑦 − 𝑧 − 𝑧 ∂2𝑢𝑧 ∂𝑥2 , ∂2𝑢𝑧 ∂𝑦2 , 2𝑒𝑥𝑦 = ∂𝑢𝑥 ∂𝑦 + ∂𝑢𝑦 ∂𝑥 − 2𝑧 ∂2𝑢𝑧 ∂𝑥 ∂𝑦 , (10.40) (10.41) (10.42) where it is understood that all quantities refer to the local element coordinate system. Substitution of Equations (10.32) into the above strain-displacement relations yields where 𝛆 = 𝐄m𝜹 − 𝑧𝐄f𝛉̂, T = {𝜀𝑥𝑥 𝛆 𝜀𝑦𝑦 2𝜀𝑥𝑦}, (10.43) (10.44) Triangular Shells LS-DYNA Theory Manual with and 𝐄m = ∂𝜙𝑥𝑖 ∂𝑥 ∂𝜙𝑦𝑖 ∂𝑦 + ⎡ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ∂𝜙𝑥𝑖 ⎢ ∂𝑦 ⎣ ⎤ ⎥ ⎥ ⎥ , ⎥ ⎥ ⎥ ∂𝜙𝑦𝑖 ⎥ ∂𝑥 ⎦ 𝐄f = ⎡ ∂2𝜙𝑧𝑖 ⎤ ⎥ ⎢ ∂𝑥2 ⎥ ⎢ ∂2𝜙𝑧𝑖 ⎥ ⎢ ⎥ ⎢ . ⎥ ⎢ ∂𝑦2 ⎥ ⎢ ⎥ ⎢ ∂2𝜙𝑧𝑖 ⎥ ⎢ ∂𝑥 ∂𝑦⎦ ⎣ (10.45) (10.46) Again, the interested reader is referred to Appendices F and G in the original work of Marchertas and Belytschko [1974] for explicit expressions of the above two matrices. 10.2.4 Nodal Force Calculations The local element forces and moments are found by integrating the local element stresses through the thickness of the element. The local nodal forces are given by 𝐟 ̂ = ∫ 𝐄mT𝛔̂ 𝑑𝑉, 𝐟 ̂T = {𝑓12, 𝑓23, 𝑓31}, 𝛔̂T = {𝜎𝑥𝑥, 𝜎𝑦𝑦, 𝜎𝑥𝑦}, (10.47) (10.48) (10.49) where the side forces and stresses are understood to all be in the local convected coordinate system. Similarly, the local moments are given by 𝐦̂ = − ∫ 𝑧 𝐄fT 𝛔̂ 𝑑𝑉, 𝐦̂T = {𝑚̂1𝑥 𝑚̂1𝑦 𝑚̂2𝑥 𝑚̂2𝑦 𝑚̂3𝑥 𝑚̂3𝑦}. (10.50) (10.51) The through-the-thickness integration portions of the above local force and moment integrals are usually performed with a 3- or 5-point trapezoidal integration. A three- point inplane integration is also used; it is inpart this three-point inplane integration that increases the operation count for this element over the 𝐶0 shell, which used one- point inplane integration with hourglass stabilization. LS-DYNA Theory Manual Triangular Shells The remaining transverse nodal forces are obtained from element equilibrium considerations. Moment equilibrium requires { 𝑓 ̂ 2𝑧 𝑓 ̂ 3𝑧 } = 2𝐴 [ −𝑥̂3 𝑦̂3 𝑥̂2 − 𝑦̂2 ] { 𝑚̂1𝑥 + 𝑚̂2𝑥 + 𝑚̂3𝑥 𝑚̂1𝑦 + 𝑚̂2𝑦 + 𝑚̂3𝑦 }, where 𝐴 is the area of the element. Next transverse force equilibrium provides 1𝑧 = −𝑓 ̂ 𝑓 ̂ 2𝑧 − 𝑓 ̂ 3𝑧. (10.52) (10.53) The corresponding global components of the nodal forces are obtained from the following transformation ⎧𝑓𝑖𝑥 ⎫ } { 𝑓𝑖𝑦 ⎬ ⎨ } { 𝑓𝑖𝑧⎭ ⎩ = 𝑓𝑖𝑗 𝑙𝑖𝑗 {⎧𝑥𝑖𝑗 + 𝑢𝑖𝑗𝑥 }⎫ 𝑦𝑖𝑗 + 𝑢𝑖𝑗𝑦 𝑧𝑖𝑗 + 𝑢𝑖𝑗𝑧 ⎭}⎬ ⎩{⎨ + 𝑓𝑖𝑘 𝑙𝑖𝑘 {⎧𝑥𝑖𝑘 + 𝑢𝑖𝑘𝑥 }⎫ 𝑦𝑖𝑘 + 𝑢𝑖𝑘𝑦 𝑧𝑖𝑘 + 𝑢𝑖𝑘𝑧 ⎭}⎬ ⎩{⎨ + 𝑓 ̂ 𝑖𝑧 {⎧𝑒3𝑥 }⎫ 𝑒3𝑦 𝑒3𝑧⎭}⎬ ⎩{⎨ . (10.54) Finally, the local moments are transformed to the body coordinates using the relation {⎧𝑚̅̅̅̅̅𝑖𝑥 }⎫ 𝑚̅̅̅̅̅𝑖𝑦 𝑚̅̅̅̅̅𝑖𝑧⎭}⎬ ⎩{⎨ = 𝛌T𝛍 {⎧𝑚̂𝑖𝑥 }⎫ 𝑚̂𝑖𝑦 𝑚̂𝑖𝑧⎭}⎬ ⎩{⎨ . (10.55) LS-DYNA Theory Manual Fully Integrated Shell (Type 16) 11 Fully Integrated Shell (Type 16) 11.1 Introduction Shell type 16 in LS-DYNA is a fully integrated shell with assumed strain interpolants used to alleviate locking and enhance in-plane bending behavior, see Engelmann, Whirley, and Goudreau [1989]; Simo and Hughes [1986]; Pian and Sumihara [1985]. It uses a local element coordinate system that rotates with the material to account for rigid body motion and automatically satisfies frame invariance of the constitutive relations. The local element coordinate system is similar to the one used for the Belytschko-Tsay element, where the the first two basis vectors are tangent to the shell midsurface at the center of the element, and the third basis vector is in the normal direction of this surface and initially coincident with the fiber vectors. 11.2 Hu-Washizu Three Field Principle The element is derived starting from the Hu-Washizu three-field principle stated as 0 = 𝛿Π(𝐯, 𝐃̅̅̅̅̅ , 𝛔̅̅̅̅̅) = ∫ 𝛿𝐃̅̅̅̅̅ : 𝛔(𝐃̅̅̅̅̅ )𝑑Ω + ∫ 𝛿[𝛔̅̅̅̅̅: (𝐃(𝐯) − 𝐃̅̅̅̅̅ )]𝑑Ω − 𝛿𝑃ext + 𝛿𝑃kin, (11.1) where 𝐯 is the velocity, 𝐃̅̅̅̅̅ is the assumed strain rate, 𝛔̅̅̅̅̅ is the assumed stress, 𝛔 denotes the constitutive update as a function of the assumed strain rate, and 𝐃 is the strain rate computed from the velocity field. 𝛿𝑃kin and 𝛿𝑃ext are the virtual power contributions from the inertial and external forces, respectively, and Ω denotes the domain of the shell element. The contribution from the internal forces can be decomposed in the in- plane and transverse shear parts as 𝑝 + 𝛿𝑃int 𝑠 + 𝐻𝑝 + 𝐻𝑠 − 𝛿𝑃ext + 𝛿𝑃kin, 0 = 𝛿𝑃int (11.2) where Fully Integrated Shell (Type 16) LS-DYNA Theory Manual p = ∫ 𝛿𝐃̅̅̅̅̅ p: 𝛔p(𝐃̅̅̅̅̅ )𝑑Ω 𝛿𝑃int , 𝛿𝑃int s = 𝜅 ∫ 𝛿𝐃̅̅̅̅̅ s: 𝛔s(𝐃̅̅̅̅̅ )𝑑Ω , 𝐻p = ∫ 𝛿[𝛔̅̅̅̅̅p: (𝐃p(𝐯) − 𝐃̅̅̅̅̅ p)]𝑑Ω , 𝐻s = 𝜅 ∫ 𝛿[𝛔̅̅̅̅̅s: (𝐃s(𝐯) − 𝐃̅̅̅̅̅ s)]𝑑Ω . (11.3) (11.4) (11.5) (11.6) Here κ is the shear correction factor and the superscripts mean that only the in-plane components (p) or transverse shear (s) components are treated. 11.3 In-plane Assumed Strain Field Using the standard isoparametric interpolation for the four-node quadrilateral element, the in-plane strain rate can be written 𝐃p = [𝐁m 𝑧𝐁b] [𝐯p 𝛉̇p], (11.7) where 𝐁m and 𝐁b are strain-displacement matrices for membrane and bending modes, respectively, 𝑧 is the through thickness coordinate and 𝐯p and 𝛉̇p are the nodal (in- plane) translational and rotational velocities, respectively. To derive the in-plane assumed strain field, the interpolants for the assumed stress and strain rates are chosen as where and 𝛔̅̅̅̅̅p = [𝐒p 𝐒p][ 𝐬m 𝐬b ], 𝐃̅̅̅̅̅ p = 𝐂−1[𝐒p 𝐒p][ 𝐞m 𝐞b ], 𝐒p = ⎡ ⎢⎢ ⎣ 2𝜂̂ 𝑎1 2𝜂̂ 𝑎2 𝑎1𝑎2𝜂̂ 2𝜉 ̂ 𝑏1 ⎤ 2𝜉 ̂ ⎥⎥ , 𝑏2 𝑏1𝑏2𝜉 ̂⎦ 𝜉 ̂ = 𝜉 − |Ω| , ∫ 𝜉𝑑Ω (11.8) (11.9) (11.10) (11.11) LS-DYNA Theory Manual Fully Integrated Shell (Type 16) 𝜂̂ = 𝜂 − |Ω| . ∫ 𝜂𝑑Ω (11.12) Furthermore, 𝐂 is the plane stress constitutive matrix and 𝜉 and 𝜂 are the isoparametric coordinates. The coefficients 𝑎𝑖 and 𝑏𝑖 are defined through 𝐉0 = [ 𝑎1 𝑎2 𝑏1 𝑏2 ], (11.13) where 𝐉0 is the area jacobian matrix from the isoparametric to physical domain computed at the element center. Inserting the expressions for the strain rate and assumed stress and strain rate into the expression for 𝐻p and requiring 𝐻p = 0 for arbitrary 𝐬m, 𝐬b, 𝐞m and 𝐞b, yields the following expression for the assumed strain rate in terms of the nodal velocities 𝐃̅̅̅̅̅ p = [𝐁̅̅̅̅̅m 𝑧𝐁̅̅̅̅̅b] [𝐯p 𝛉̇p], (11.14) where and 𝐁̅̅̅̅̅m = 𝐂−1𝐒p𝐄̂𝐁̂m, 𝐁̅̅̅̅̅b = 𝐂−1𝐒p𝐄̂𝐁̂b, 𝐄̂ = ∫ 𝐒pT𝐂−1𝐒p𝑑Ω , 𝐁̂m = ∫ 𝐒pT𝐁m𝑑Ω , 𝐁̂b = ∫ 𝐒pT𝐁b𝑑Ω . (11.15) (11.16) (11.17) (11.18) (11.19) 11.4 Transverse Shear Assumed Strain Field The transverse shear strain is the Bathe-Dvorkin [1984] assumed natural strain field and is derived as follows. Using the standard isoparametric interpolation for the four-node quadrilateral element, the transverse shear strain rate can be written 𝐯𝑧 𝛉̇𝑝], where 𝐁𝑡 is the corresponding strain-displacement matrix and 𝐯𝑧 and 𝛉̇𝑝 are the nodal out-of-plane translational and in-plane rotational velocities, respectively. 𝐃s = 𝐁𝑡[ (11.20) The assumed strain rate is defined as Fully Integrated Shell (Type 16) LS-DYNA Theory Manual where 𝐃̅̅̅̅̅ s = 𝐁̅̅̅̅̅𝑡[ 𝐯𝑧 𝛉̇p], 𝐁̅̅̅̅̅𝑡 = 𝐉−T𝐄 ∫ 𝐒𝑠T𝐉T𝐁𝑡𝑑Ω , (11.21) (11.22) Here 𝐉 is the area jacobian matrix from the isoparametric domain to the physical domain, 𝐄 = [ 1 − 𝜉 1 + 𝜉 1 − 𝜂 1 + 𝜂 ], 𝐒s = [ δ(η)δ(1 + ξ) δ(η)δ(1 − ξ) δ(ξ)δ(1 + η) δ(ξ)δ(1 − η) ], (11.23) (11.24) and 𝛿 is the Dirac delta function. Defining the assumed stress as 𝛔̅̅̅̅̅p = 𝐉𝐒s𝐬, (11.25) yields 𝐻s = 0 regardless of the choice of 𝐬 and thus a B-bar expression for the assumed transverse strain rates is obtained as given above. The result is equivalent to defining the isoparametric assumed shear strain rates by interpolating the corresponding strain rates from the mid-side points A, B, C and D shown in Figure 11.1. Figure 11.1. Midside locations of isoparametric strain rates LS-DYNA Theory Manual Fully Integrated Shell (Type 16) 11.5 Rigid Body Motion For the in-plane assumed strain field, a rigid body motion may induce a nonzero strain rate. The expression for the in-plane strain rate for a rigid body motion is 𝐃̅̅̅̅̅ r = 𝐁̅̅̅̅̅r𝛉̇, where 𝐁̅̅̅̅̅r = 𝑤𝐁̅̅̅̅̅m𝐑. (11.26) (11.27) 11.6 Belytschko-Leviathan Projection For warped configurations and since the geometry of the current shell element is flat, extremely flexible behavior can be expected for some modes of deformation. Following [Belytschko and Leviathan 1994], a 7-mode projection matrix 𝐏 (3 rigid body rotation modes and 4 nodal drill rotation modes) is constructed used for projecting out these zero energy modes. The explicit formula for the projection matrix is given by 𝐏 = 𝐈 − 𝐑(𝐑T𝐑)−1𝐑T, (11.28) where 𝐑 is a matrix where each column corresponds to the nodal velocity of a zero energy mode. This projection matrix operates on the nodal velocities prior to computing the strain rates, and also on the resulting internal force vector to maintain invariance of the internal power. LS-DYNA Theory Manual Shells with Thickness Stretch 12 Shells with Thickness Stretch 12.1 Introduction Thickness stretch is of considerable importance in problems involving finite thickness strains, contact and surface loads in nonlinear shell applications. As an example, in sheet metal forming applications, the presence of normal stresses in thickness direction improves the accuracy of the solution and also its response on the double sided contact zone between dies and sheet. It has also been shown that a kinematical representation of a continuous thickness field improves the instability characteristics when compared to experimental results, see Figure Figure 1212-1 and Björklund [2014]. There have been several attempts to account for the through-thickness deformation in the literature, this implementation is inspired by the 7P-CYSE shell introduced in Cardoso and Yoon [2005]. However, the formulation in this paper is rather complicated and involves for instance assumed shear strains (ANS) to alleviate shear locking and complicated setup of internal forces and stiffness matrices by combined analytical and numerical integration to restore rank deficiencies. A direct implementation of this shell following the theory was ruled out for efficiency reasons, and another approach was taken in order to presumably get a useful shell. The Belytschko-Tsay shell element is one of the fastest elements for thin shell simulations. This, together with its robustness, is the reason why it is popular in finite element codes. The implementation of shell type 25, the reduced integrated shell with thickness stretch, is based on the formulation of the Belytschko-Tsay shell with a relaxation of the thickness variable. This ensures that it will be efficient and hopefully also possess properties useful for applications where through thickness deformation is important. As a fully integrated alternative, shell type 26 is available as an analogue extension of shell type 16 (fully integrated Belytschko-Tsay), and a triangular shell with thickness stretch is available as type 27 mainly to allow for hybrid meshes (quadrilat- erals combined with triangles) in this context. The theory that follows is very similar to that of the Belytschko-Tsay (type 2), Fully Integrated Shell (type 16) and C0-shell (type 4), and here we emphasize on the parts involving the amendments to those shell formulations. Shells with Thickness Stretch LS-DYNA Theory Manual Shell 16, no transverse shear discontinuous and stress thickness field Shell 26, transverse shear stress and continuous thickness field 25 20 15 10 ] [ , 0.5 Experiment Plane Stress With Normal Stress 2.5 1.5 Displacement, δ [mm] Figure 1212-1 Example of premature localization with shell type 16 while shell type 26 matches experimental result (from Björklund 12.2 Shell Type 25 12.2.1 Formulation The kinematics, i.e., position 𝒙 and velocity 𝒗, of a material point in the shell with through thickness stretch can be written in the shell element local coordinate system as (sum over nodal indices 𝐼) where we have set 𝒙 = (𝒙𝐼 + 𝑠𝐼𝒏)𝑁𝐼(𝜉 , 𝜂) 𝒗 = (𝒗𝐼 + 𝑠𝐼𝝎𝐼 × 𝒏 + 𝑠 ̇𝐼𝒏)𝑁𝐼(𝜉 , 𝜂) 𝑠𝐼 = 𝑡𝐼 + (1 − 𝜍2)𝑞𝐼. (12.1) (12.2) The kinematics is based on the Belytschko-Tsay shell with the additional feature that the thickness is variable, whence the last term in the second of (12.1). The thickness variable is represented by 𝑡𝐼 and an additional strain variable 𝑞𝐼 to allow for a linear strain through the thickness. The latter represents the location of the mid-surface and is important to avoid “Poisson locking” in bending modes of deformation, so the shell has two additional degrees of freedom compared to the Belytschko-Tsay shell. The other variables and parameters are the nodal coordinates 𝒙𝐼, nodal velocities 𝒗𝐼, nodal 1)𝑇 and bilinear isoparametric shape rotational velocities 𝝎𝐼, shell normal 𝒏 = (0 functions 𝑁𝐼. From this we can determine the local velocity gradient as 𝜕𝒗 𝜕𝒙 = (𝒗𝐼 + 𝑠𝐼𝝎𝐼 × 𝒏 + 𝑠 ̇𝐼𝒏) 𝜕𝑁𝐼 𝜕𝒙 + (𝝎𝐼 × 𝒏 𝜕𝑠𝐼 𝜕𝒙 + 𝒏 𝜕𝑠 ̇𝐼 𝜕𝒙 ) 𝑁𝐼. (12.3) LS-DYNA Theory Manual Shells with Thickness Stretch In the local system one can assume a vanishing third component of both 𝝎𝐼 × 𝒏 and and the thickness strain rate is given by 𝜕𝑁𝐼 𝜕𝒙 , 𝜀̇𝑡 = 𝜕𝑠 ̇ 𝜕𝑥3 = 𝑡 ̇− 4𝜍𝑞 ̇ 𝑡 − 4𝜍𝑞 (12.4) where we used the notation 𝑠 = 𝑠𝐼𝑁𝐼, 𝑡 = 𝑡𝐼𝑁𝐼 and 𝑞 = 𝑞𝐼𝑁𝐼, sum over 𝐼. For small strains 𝑞 = 0, and this shows that the thickness strain rate is at most linear. For evaluating internal forces we define the strain-displacement tensor through (assuming Voigt notation and sum over 𝐼) 𝜕𝒗 𝜕𝒙 = 𝑩𝐼𝒖𝐼 , (12.5) and the nodal vector 𝒖𝐼 is given by 𝑡 ̇𝐼 indicating the 8 degrees of freedom per node in these elements. The principle of virtual work results in an internal force vector 𝒖𝐼 = (𝒗𝐼 𝑇 𝝎𝐼 𝑞 ̇𝐼)𝑇 , (12.6) 𝒇𝐼 = ∫ 𝑩𝐼 𝑇𝝈 , (12.7) where 𝝈 is the Cauchy stress and the integral is over the current element configuration. 12.2.2 Hourglass modes Shell type 25 is a reduced integration element and in addition to the six hourglass modes present in the original Belytschko-Tsay shell, two more are added by the introduction of the thickness variables. Fortunately these are orthogonal to any rigid body motion and/or any other hourglass mode, and are given by where 𝑡𝐼 = ℎ𝐼 𝑞𝐼 = ℎ𝐼 ℎ𝐼 = (−1)𝐼/4 (12.8) (12.9) and all other displacement components are zero. To restrain these modes we have included generalized strains and stresses according to the following (sum over 𝐼) ℎ = 𝜀̇𝑡 ℎ = − 𝜀̇𝑞 ℎ𝐼𝑡 ̇𝐼 4ℎ𝐼𝑞 ̇𝐼 The corresponding generalized stresses are obtained through 𝜎̇𝑡 = 𝐸𝐻𝜀̇𝑡 (12.10) (12.11) Shells with Thickness Stretch LS-DYNA Theory Manual and the forces are then given by 𝜎̇𝑞 = 𝐸𝐻 𝜀̇𝑞 𝑡 = 𝐴ℎ𝐼𝜎𝑡 𝑓𝐼 𝑞 = −4𝐴ℎ𝐼𝜎𝑞 𝑓𝐼 (12.12) where 𝐴 is the area of the element and the value of 𝐸𝐻 is taken as 𝐸𝐻 = 0.05𝐸, i.e., 5% of the Young’s modulus. 12.3 Shell Type 26 12.3.1 Modifying shell type 16 When using full integration, care must be taken in order to avoid the well-known shear locking phenomenon. Common techniques developed for this are the ANS (Assumed Natural Strain) and various types of EAS (Enhanced Assumed Strain) techniques. In Cardoso and Yoon [2004] the ANS technique is used in which the transverse shear strains are interpolated from the mid points of the shell element edges. It is reported that this is a successful technique, but when consulting Bischoff and Ramm [1997] it is reported that it is not well suited to avoid membrane locking and reduce mesh distortion sensitivity. They are proposing a combination of ANS and EAS to get a decent shell element formulation. However, elements that use an EAS in general require a nonlinear solution for the assumed strain variables which can be computa- tionally rather expensive. The approach taken here is to suitably modifying an existing LS-DYNA standard assumed strain element, i.e., element type 16, which is a fully integrated extension of the Belytschko-Tsay element. Due to the rather complex setup of assumed strain components, we use the following in order to extend the element to variable thickness stretch without having to bother about all the details of the kinematics. In the beginning of a time step, the thickness components are reset to the corresponding value in the center of the shell element. That is 𝑠 ̃ = 𝑠1 + 𝑠2 + 𝑠3 + 𝑠4 (12.13) is used for evaluating the strain increments. However, the rates of the thickness variables are unchanged, so this can be seen as an assumed strain approach in the thickness direction. Using this, the velocity gradient expression is an augmentation of that of element 16 𝜕𝒗 𝜕𝒙 = 𝜕𝒗 𝜕𝒙 ∣ 16 + 𝑠 ̇𝐼𝒏 𝜕𝑁𝐼 𝜕𝒙 + 𝒏 𝜕𝑠 ̇𝐼 𝜕𝒙 𝑁𝐼. (12.14) This should be interpreted that the velocity gradient used in shell element type 16 as a function of the current thickness coordinate 𝑠 ̃ (and its isoparametric derivative) is LS-DYNA Theory Manual Shells with Thickness Stretch augmented by thickness component rates. Furthermore, to avoid locking phenomena and still maintaining a non-singular element we use single point integration of the thickness strain component and an ANS approach for the transverse shear strain components emanating from the rates of thickness components. This approach is inspired by the methodology used for the Belytschko-Tsay shell in which the nodal fiber vectors are reset in the beginning of each time step, and in an analogous way we reset the thickness components in the beginning of each time step in this shell element formulation. 12.4 Shell Type 27 12.4.1 Modifying shell type 4 A triangular element with thickness stretch was added to allow consistent sorting of triangular shell elements, and not necessarily intended to be used for other purposes. The approach taken is very similar to that of shell type 26, the existing LS-DYNA standard C0 triangular element was modified according to the same principles as described in the previous section. In this case the velocity gradient expression is modified according to 𝜕𝒗 𝜕𝒙 = 𝜕𝒗 𝜕𝒙 ∣ + 𝒏 𝜕𝑠 ̃ 𝜕𝒙 (12.15) where again the subindex 4 indicates that it’s the velocity gradient of element type 4 evaluated with respect to the average thickness value 𝑠 ̃ and its isoparametric derivative. For the triangular element type 27 the thickness is always constant in the element, a decision that was taken for the sake of simplicity. More on thickness distribution in the next section. 12.5 Related Features 12.5.1 Continuous vs decoupled thickness field A drawback with having a continuous thickness field is that complicated geometries tend to lock the structure. This approach assumes that the geometry is relatively flat and may be suitable in metal forming but not in other situations. To remedy this we added the option to decouple the thickness field so that the thickness is discontinuous between elements, which makes the element suitable for crash analysis. To activate this option the user should put the variable IDOF on *SECTION_SHELL equal to 2, which actually is the default. For shell element type 25, this option will make the thickness variable constant in the element, and the implementation follows the one described above with the restriction 𝑡𝐼 = 𝑡 (constant) and 𝑞𝐼 = 𝑞 (constant). No additional zero energy modes are present with this approach. LS-DYNA Draft Shells with Thickness Stretch LS-DYNA Theory Manual Using the same approach for element type 26 turns out to be a poor choice since it leads to locking phenomenon due to full integration. Instead we use the approach where the thickness is bilinear within but discontinuous between elements, which turns out to be successful. That means that the same code can be executed regardless of the choice of IDOF for this element. 12.5.2 Nodal masses For dynamic analysis some mass quantity must be associated with the extra degrees of freedom, and although a consistent finite element approach is applicable the mass is here empirically estimated from elaborating with the kinetic energy for compressive in- plane and out-of-plane modes. That is, the kinetic energy of an in-plane uniaxial strain mode should have the same kinetic energy as the equivalent out-of-plane ditto. This assumption leads to a mass of the scalar nodes given by 𝑚 = 𝑚𝑇/4 where 𝑚𝑇 is the translational mass. A problem with this approach is that it leads to instabilities due to high eigenfrequencies of the shell. For this reason we have set 3𝐴 2𝑡2)𝑚𝑇 where 𝐴 is the element area and 𝑡 is the thickness. 𝑚 = max(1, 𝒇 (12.16) 𝑡 Figure 1212-2 Contact influence on thickness stretch shells. −𝒇 12.5.3 Transfer of contact forces The new degrees of freedom allows for a different treatment of how contact forces are transferred from master to slave, for this discussion we refer to Figure Figure 1212-2. The nodal forces in local system acting on the slave from contact on the upper and lower surface can roughly be written LS-DYNA Theory Manual Shells with Thickness Stretch 𝑢/𝑙 = (± 𝒇𝐼 𝒇 𝑇 (𝒏 × ) 𝑇 𝒏 ∙ 𝒇 0) (12.17) where we used the same order of the degrees of freedom as in (12.6). Summing these two force contributions give nodal contact forces acting on the slave given by 𝑐 = (𝟎𝑇 𝒇𝐼 𝑡 (𝒏 × ) 𝑇 𝒏 ∙ 𝒇 0) (12.18) We can see that the total force include nodal moments caused by the frictional forces acting at an offset from the midsurface of the shell, but also a pressure acting on the thickness degree of freedom. In conclusion, the relaxation of the thickness in the Belytschko-Tsay shell allows for double sided contact zones, i.e., the shell is affected by contact pressure from both sides even though they are of equal magnitude. This is not possible in traditional shell with zero normal stress, unless a modified option is used. 12.6 Contact Pressure Treatment in Shells 2, 4 and 16 By specifying IDOF = 3 on *SECTION_SHELL for the Belytschko-Tsay (type 2), C0- element (type 4) and Fully Integrated (type 16) shell, the contact pressure influences the stress and can induce thickness changes. This is a short explanation of the theory behind. The z-stress in a shell element is usually restricted to be zero, but in this case we intend to solve the constitutive update using the constraint where and 𝜎𝑧𝑧 = 𝛼𝜎𝑐(𝑧) 𝜎𝑐(𝑧) = − 𝑏 − 𝜎𝑐 𝜎𝑐 (𝑧3 − 3𝑧) − 𝑏 + 𝜎𝑐 𝜎𝑐 (12.19) (12.20) 𝑏= contact pressure at bottom surface of shell 𝑡= contact pressure at top surface of shell 𝜎𝑐 𝜎𝑐 𝑧= isoparametric coordinate through the thickness between -1 and 1 𝛼= scaling parameter The scaling parameter can be set as *CONTROL_CONTACT. The constitutive update for en elastic-plastic material can be written the 8th parameter on card 3 on 𝛔𝑛+1 = 𝛔𝑛 + 𝐾∆𝜀𝑣𝑜𝑙𝐈 + ∆𝐬(𝐬𝑛, ∆𝛆𝑑𝑒𝑣) 𝑛+1 = 𝜎𝑐 𝜎𝑧𝑧 𝑛+1 (12.21) (12.22) where Shells with Thickness Stretch LS-DYNA Theory Manual 𝛔𝑛+1 = stress in step n+1 𝛔𝑛 = stress in step n 𝐾= bulk modulus ∆𝛆 = strain increment ∆𝜀𝑣𝑜𝑙 = ∆𝛆: 𝐈 = volumetric strain increment 𝐈 = unit tensor ∆𝐬= deviatoric stress increment 𝐬𝑛 = 𝛔𝑛 − 𝛔𝑛:𝐈 ∆𝛆𝑑𝑒𝑣 = ∆𝛆 − ∆𝛆: 𝐈 3 𝐈 = deviatoric stress in step n 3 𝐈 = deviatoric strain increment The independent variables in (12.21) and (12.22) are 𝜎𝑥𝑥 ∆𝜀𝑧𝑧. Here we assume that the stress response can be decoupled into a volumetric and deviatoric part and the deviatoric stress increment depends only on the deviatoric part of the stress and strain increment as indicated in the formula. We can rewrite (12.21) and (12.22) as 𝑛+1, 𝜎𝑦𝑦 𝑛+1, 𝜎𝑥𝑦 𝑛+1, 𝜎𝑦𝑧 𝑛+1 and 𝑛+1, 𝜎𝑥𝑧 by substituting and 𝛔̃𝑛+1 = 𝛔̃𝑛 + 𝐾∆𝜀̃𝑣𝑜𝑙𝐈 + ∆𝐬(𝐬̃𝑛, ∆𝛆̃𝑑𝑒𝑣) 𝑛+1 = 0 𝜎̃𝑧𝑧 𝑛𝐈 𝛔̃𝑛 = 𝛔𝑛 − 𝜎𝑐 𝛔̃𝑛+1 = 𝛔𝑛+1 − 𝜎𝑐 𝑛+1𝐈 ∆𝛆̃ = ∆𝛆 − 𝑛+1 − 𝜎𝑐 𝜎𝑐 3𝐾 𝐈. Since the deviatoric stress and strain increment is not changed, i.e., 𝐬𝑛 = 𝐬̃𝑛 ∆𝛆𝑑𝑒𝑣 = ∆𝛆̃𝑑𝑒𝑣 (12.23) (12.24) (12.25) (12.26) (12.27) (12.28) (12.29) with this substitution it follows that the existing material routines can be used for 𝑛+1 and ∆𝜀̃𝑧𝑧 and then use 𝑛+1, 𝜎̃𝑦𝑦 solving (12.23) and (12.24) in terms of 𝜎̃𝑥𝑥 the inverse of (12.26) and (12.27) to establish the stress and through thickness strain increment. Thus, the algorithm is as follows 𝑛+1, 𝜎̃𝑥𝑦 𝑛+1, 𝜎̃𝑦𝑧 𝑛+1, 𝜎̃𝑥𝑧 𝑛+1 𝑛 and 𝜎𝑐 1.Given 𝛔𝑛, ∆𝛆, 𝜎𝑐 2.Use (12.25) and (12.27) to compute 𝛔̃𝑛 and ∆𝛆̃. 3.Do a constitutive update, (12.23) and (12.24), to get 𝛔̃𝑛+1 and ∆𝜀̃𝑧𝑧. 4.Use (12.26) and (12.27) to compute 𝛔𝑛+1 and ∆𝜀𝑧𝑧. LS-DYNA Theory Manual Shells with Thickness Stretch Figure 1212-3 Compression of a shell sheet between two rigid plates using IDOF = 3 on shell 16. LS-DYNA Theory Manual Hughes-Liu Shell 13 Hughes-Liu Shell The Hughes-Liu shell element formulation ([Hughes and Liu 1981a, b], [Hughes et al., 1981], [Hallquist et al., 1985]) was the first shell element implemented in LS- DYNA. It was selected from among a substantial body of shell element literature because the element formulation has several desirable qualities: • it is incrementally objective (rigid body rotations do not generate strains), allowing for the treatment of finite strains that occur in many practical applica- tions; • it is simple, which usually translates into computational efficiency and robust- ness; • it is compatible with brick elements, because the element is based on a degener- ated brick element formulation. This compatibility allows many of the efficient and effective techniques developed for the DYNA3D brick elements to be used with this shell element; • it includes finite transverse shear strains; • a through-the-thickness thinning option is also available when needed in some shell element applications. The remainder of this section reviews the Hughes-Liu shell element (referred to by Hughes and Liu as the U1 element) which is a four-node shell with uniformly reduced integration, and summarizes the modifications to their theory as it is implemented in LS-DYNA. A detailed discussion of these modifications, as well as those associated with the implementation of the Hughes-Liu shell element in NIKE3D, are presented in an article by Hallquist and Benson [1986]. Hughes-Liu Shell LS-DYNA Theory Manual 13.1 Geometry The Hughes-Liu shell element is based on a degeneration of the standard 8-node brick element formulation, an approach originated by Ahmad et al. [1970]. Recall from the discussion of the solid elements the isoparametric mapping of the biunit cube: 𝐱(𝜉 , 𝜂, 𝜁 ) = 𝑁𝑎(𝜉 , 𝜂, 𝜁 )𝐱𝑎, 𝑁𝑎 (𝜉 , 𝜂, 𝜁 ) = (1 + 𝜉𝑎𝜉 )(1 + 𝜂𝑎𝜂)(1 + 𝜁𝑎𝜁 ) , (13.1) (13.2) where 𝐱 is an arbitrary point in the element, (𝜉 , 𝜂, 𝜁 ) are the parametric coordinates, 𝐱𝑎 are the global nodal coordinates of node 𝑎, and 𝑁𝑎 are the element shape functions evaluated at node 𝑎, i.e., (𝜉𝑎, 𝜂𝑎, 𝜁𝑎) are (𝜉 , 𝜂, 𝜁 ) evaluated at node 𝑎. In the shell geometry, planes of constant 𝜁 will define the lamina or layers of the shell and fibers are defined by through-the-thickness lines when both 𝜉 and 𝜂 are constant (usually only defined at the nodes and thus referred to as ‘nodal fibers’). To degenerate the 8-node brick geometry into the 4-node shell geometry, the nodal pairs in the 𝜁 direction (through the shell thickness) are combined into a single node, for the translation degrees of freedom, and an inextensible nodal fiber for the rotational degrees of freedom. Figure 13.1 shows a schematic of the bi-unit cube and the shell element. The mapping of the bi-unit cube into the shell element is separated into two parts 𝐱(𝜉 , 𝜂, 𝜁 ) = 𝐱̅(𝜉 , 𝜂) + 𝐗(𝜉 , 𝜂, 𝜁 ), (13.3) where 𝐱̅ denotes a position vector to a point on the reference surface of the shell and X is a position vector, based at point 𝐱̅ on the reference, that defines the fiber direction through that point. In particular, if we consider one of the four nodes which define the reference surface, then 𝐱̅ (𝜉 , 𝜂) = 𝑁𝑎 (𝜉 , 𝜂) 𝐱̅𝑎, 𝐗(𝜉 , 𝜂, 𝜁 ) = 𝑁𝑎 (𝜉 , 𝜂)𝐗𝑎(𝜁 ). (13.4) (13.5) With this description, arbitrary points on the reference surface 𝐱̅ are interpolated by the two-dimensional shape function 𝑁(𝜉 , 𝜂) operating on the global position of the four shell nodes that define the reference surfaces, i.e., 𝐱̅𝑎. Points off the reference surface are further interpolated by using a one-dimensional shape function along the fiber direction, i.e., 𝐗𝑎(𝜁 ), where 𝐗𝑎(𝜁 ) = 𝑧𝑎(𝜁 ) 𝐗̂𝑎, 𝑧𝑎(𝜁 ) = 𝑁+(𝜁 )𝑧𝑎 −, + + 𝑁−(𝜁 )𝑧𝑎 (13.6) (13.7) LS-DYNA Theory Manual Hughes-Liu Shell Biunit Cube Beam Element Nodal fibers Top Surface z+ x+ x^ x¯ x^ x- Bottom Surface z- +1 ζ¯ -1 Figure 13.1. Mapping of the biunit cube into the Hughes-Liu shell element and nodal fiber nomenclature. 𝑁+(𝜁 ) = 𝑁−(𝜁 ) = (1 + 𝜁 ) , (1 − 𝜁 ) (13.8) (13.9) As shown in the lower portion of Figure 13.1, 𝐗̂𝑎 is a unit vector in the fiber direction and 𝑧(𝜁 ) is a thickness function. (Thickness changes are accounted for by explicitly adjusting the fiber lengths at the completion of a time step based on the amount of straining in the fiber direction. Updates of the fiber lengths always lag one time step behind other kinematical quantities.) The reference surface may be located at the mid-surface of the shell or at either of the shell’s outer surfaces. This capability is useful in several practical situations involving contact surfaces, connection of shell elements to solid elements, and offsetting elements such as stiffeners in stiffened shells. The reference surface is located within the shell element by specifying the value of the parameter 𝜁 ̅ (see lower portion of Figure Hughes-Liu Shell LS-DYNA Theory Manual 13.1). When 𝜁 ̅ = – 1, 0, +1, the reference surface is located at the bottom, middle, and top surface of the shell, respectively. The Hughes-Liu formulation uses two position vectors, in addition to 𝜁 ̅, to locate + the reference surface and define the initial fiber direction. The two position vectors 𝑥𝑎 − are located on the top and bottom surfaces, respectively, at node 𝑎. From these and 𝑥𝑎 data the following are obtained: 𝑥̅𝑎 = (1 − 𝜁 ̅)𝑥𝑎 +, − + (1 + 𝜁 ̅)𝑥𝑎 𝑋̂𝑎 = (𝑥𝑎 −) + − 𝑥𝑎 ℎ𝑎 , + = 𝑧𝑎 (1 − 𝜁 ̅)ℎ𝑎, − = − 𝑧𝑎 (1 + 𝜁 ̅)ℎ𝑎, ℎ𝑎 = ∥𝑥𝑎 + − 𝑥𝑎 −∥, (13.10) (13.11) (13.12) (13.13) (13.14) where ‖ ⋅ ‖ is the Euclidean norm. 13.2 Kinematics The same parametric representation used to describe the geometry of the shell element, i.e., reference surface and fiber vector interpolation, are used to interpolate the shell element displacement, Again, the displacements are separated into the reference surface displacements and rotations associated with the fiber direction: isoparametric representation. i.e., an 𝐮(𝜉 , 𝜂, 𝜁 ) = 𝐮̅̅̅̅(𝜉 , 𝜂) + 𝐔(𝜉 , 𝜂, 𝜁 ), 𝐮̅̅̅̅(𝜉 , 𝜂) = 𝑁𝑎(𝜉 , 𝜂)𝐮̅̅̅̅𝑎, 𝐔(𝜉 , 𝜂, 𝜁 ) = 𝑁𝑎(𝜉, 𝜂)𝐔𝑎(𝜁 ), 𝐔𝑎(𝜁 ) = 𝑧𝑎(𝜁 )𝐔̂𝑎, (13.15) (13.16) (13.17) (13.18) where 𝐮 is the displacement of a generic point; 𝐮̅̅̅̅ is the displacement of a point on the reference surface, and 𝐔 is the ‘fiber displacement’ rotations; the motion of the fibers can be interpreted as either displacements or rotations as will be discussed. LS-DYNA Theory Manual Hughes-Liu Shell Hughes and Liu introduce the notation that follows, and the associated schematic shown in Figure 13.2, to describe the current deformed configuration with respect to the reference configuration: 𝐲 = 𝐲̅̅̅̅ + 𝐘, 𝐲̅̅̅̅ = 𝐱̅ + 𝐮̅̅̅̅, 𝐲̅̅̅̅𝑎 = 𝐱̅𝑎 + 𝐮̅̅̅̅𝑎, 𝐘 = 𝐗 + 𝐔, 𝐘𝑎 = 𝐗𝑎 + 𝐔𝑎, 𝐘̂𝑎 = 𝐗̂𝑎 + 𝐔̂𝑎. (13.19) (13.20) (13.21) (13.22) (13.23) (13.24) In the above relations, and in Figure 13.2, the 𝐱 quantities refer to the reference configuration, the 𝐲 quantities refer to the updated (deformed) configuration and the 𝐮 quantities are the displacements. The notation consistently uses a superscript bar (⋅ ̅) to indicate reference surface quantities, a superscript caret (⋅ ̂) to indicate unit vector quantities, lower case letters for translational displacements, and upper case letters indicating fiber displacements. To update to the deformed configuration, two vector quantities are needed: the reference surface displacement 𝐮̅̅̅̅ and the associated nodal fiber displacement 𝐔. The nodal fiber displacements are defined in the fiber coordinate system, described in the next subsection. 13.2.1 Fiber Coordinate System For a shell element with four nodes, the known quantities will be the displacements of the reference surface 𝐮̅̅̅̅ obtained from the translational equations of motion and some rotational quantities at each node obtained from the rotational equations of motion. To complete the kinematics, we now need a relation between nodal rotations and fiber displacements 𝐔. Hughes-Liu Shell LS-DYNA Theory Manual (parallel construction) u¯ reference axis in undeformed geometry Deformed Configuration Reference Surface x¯ Figure 13.2. Schematic of deformed configuration displacements and position vectors. At each node a unique local Cartesian coordinate system is constructed that is used as the reference frame for the rotation increments. The relation presented by Hughes and Liu for the nodal fiber displacements (rotations) is an incremental relation, i.e., it relates the current configuration to the last state, not to the initial configuration. 𝑓 ) comprising the orthonormal Figure 13.3 shows two triads of unit vectors: (𝐛1 𝑓 ) and fiber basis in the reference configuration (where the fiber unit vector is now 𝐘̂ = 𝐛3 (𝐛1, 𝐛2, 𝐛3) indicating the incrementally updated current configuration of the fiber and vectors. The reference triad is updated by applying the incremental rotations, Δ𝜃1 𝑓 ) Δ𝜃2, obtained from the rotational equations of motion, to the fiber vectors (𝐛 1 as shown in Figure 13.3. The linearized relationship between the components of Δ𝑈̂ in the fiber system viz, Δ𝑈̂ 𝑓 , and the incremental rotations is given by 𝑓 and 𝐛 2 𝑓 , Δ𝑈̂ 𝑓 , 𝐛2 𝑓 , 𝐛3 𝑓 , Δ𝑈̂ ⎧Δ𝑈̂ {{ Δ𝑈̂ ⎨ {{ Δ𝑈̂ ⎩ ⎫ }} ⎬ }} ⎭ = −1 ⎢⎡ ⎣ 0 −1 0 ⎦ ⎥⎤ { Δ𝜃1 Δ𝜃2 }. (13.25) Although the above Hughes-Liu relation for updating the fiber vector enables a reduction in the number of nodal degrees of freedom from six to five, it is not implemented in LS-DYNA because it is not applicable to beam elements. LS-DYNA Theory Manual Hughes-Liu Shell fiber ^ f =Y b3 b3 Δθ b1 b1 b2 b2 Δθ Figure 13.3. incremental rotations. Incremental update of fiber vectors using Hughes-Liu In LS-DYNA, three rotational increments are used, defined with reference to the global coordinate axes: {{⎧Δ𝑈̂1 }}⎫ Δ𝑈̂2 }}⎬ ⎩{{⎨ Δ𝑈̂3⎭ = 𝑌̂3 −𝑌̂2 ⎤ ⎡ −𝑌̂3 𝑌̂1 ⎥⎥ ⎢⎢ 𝑌̂2 −𝑌̂1 0 ⎦ ⎣ {⎧Δ𝜃1 }⎫ Δ𝜃2 Δ𝜃3⎭}⎬ ⎩{⎨ . (13.26) Equation (13.26) is adequate for updating the stiffness matrix, but for finite rotations the error is significant. A more accurate second-order technique is used in LS- DYNA for updating the unit fiber vectors: 𝑌̂ 𝑛+1 = 𝑅𝑖𝑗(Δ𝜃)𝑌̂𝑖 𝑛, 𝑅𝑖𝑗(Δ𝜃) = 𝛿𝑖𝑗 + (2𝛿𝑖𝑗 + Δ𝑆𝑖𝑘)Δ𝑆𝑖𝑘 , ΔS𝑖𝑗 = e𝑖𝑘𝑗Δ𝜃𝑘, 2𝐷 = 2 + (Δ𝜃1 2 + Δ𝜃2 2 + Δ𝜃3 2). (13.27) (13.28) (13.29) (13.30) Here, 𝛿𝑖𝑗 is the Kronecker delta and 𝑒𝑖𝑗𝑘 is the permutation tensor. This rotational update is often referred to as the Hughes-Winget formula [Hughes and Winget 1980]. An exact rotational update using Euler angles or Euler parameters could easily be substituted in Equation (13.27), but it is doubtful that the extra effort would be justified. 13.2.2 Lamina Coordinate System In addition to the above described fiber coordinate system, a local lamina coordinate system is needed to enforce the zero normal stress condition, i.e., plane Hughes-Liu Shell LS-DYNA Theory Manual nt nsta ξ = co e^ η = constant e^ e^ Figure 13.4. Schematic of lamina coordinate unit vectors. stress. Lamina are layers through the thickness of the shell that correspond to the locations and associated thicknesses of the through-the-thickness shell integration points; the analogy is that of lamina in a fibrous composite material. The orthonormal lamina basis (Figure 13.4), with one direction 𝑒 ̂3 normal to the lamina of the shell, is constructed at every integration point in the shell. The lamina basis is constructed by forming two unit vectors locally tangent to the lamina: 𝐞̂1 = 𝐞′2 = 𝐲,𝜉 ∥𝐲,𝜉 ∥ , 𝐲,𝜂 ∥𝐲,𝜂 ∥ , (13.31) (13.32) where, as before, 𝐲 is the position vector in the current configuration. The normal to the lamina at the integration point is constructed from the vector cross product of these local tangents: 𝐞̂3 = 𝐞̂1 × 𝐞′2, 𝐞̂2 = 𝐞̂3 × 𝐞̂1, (13.33) (13.34) is defined, because 𝐞̂2, although tangent to both the lamina and lines of constant 𝜉 , may not be normal to 𝐞̂1 and 𝐞̂3. The lamina coordinate system rotates rigidly with the element. The transformation of vectors from the global to lamina coordinate system can now be defined in terms of the lamina basis vectors as ⎧𝐴̂𝑥 ⎫ }} {{ 𝐴̂𝑦 ⎬ ⎨ }} {{ 𝐴̂𝑧⎭ ⎩ 𝑒3𝑥 𝑒2𝑥 𝑒1𝑥 ⎥⎤ ⎢⎡ 𝑒1𝑦 𝑒2𝑦 𝑒3𝑦 𝑒3𝑧 ⎦ 𝑒2𝑧 𝑒1𝑧 ⎣ {⎧𝐴𝑥 }⎫ 𝐴𝑦 𝐴𝑧⎭}⎬ ⎩{⎨ 𝐀̂ = = = 𝐪𝐀, (13.35) LS-DYNA Theory Manual Hughes-Liu Shell where 𝑒𝑖𝑥, 𝑒𝑖𝑦, 𝑒𝑖𝑧 are the global components of the lamina coordinate unit vectors; 𝐀̂ is a vector in the lamina coordinates, and 𝐴 is the same vector in the global coordinate system. 13.3 Strains and Stress Update 13.3.1 Incremental Strain and Spin Tensors The strain and spin increments are calculated from the incremental displacement gradient 𝐺𝑖𝑗 = ∂Δ𝑢𝑖 ∂𝑦𝑗 , (13.36) where Δ𝑢𝑖 are the incremental displacements and 𝑦𝑗 are the deformed coordinates. The incremental strain and spin tensors are defined as the symmetric and skew-symmetric parts, respectively, of 𝐺𝑖𝑗: Δ𝜀𝑖𝑗 = Δ𝜔𝑖𝑗 = (𝐺𝑖𝑗 + 𝐺𝑗𝑖), (𝐺𝑖𝑗 − 𝐺𝑗𝑖). (13.37) (13.38) The incremental spin tensor Δ𝜔𝑖𝑗 is used as an approximation to the rotational contribution of the Jaumann rate of the stress tensor; LS-DYNA implicit uses the more accurate Hughes-Winget transformation matrix (Equation (13.27)) with the incremental spin tensor for the rotational update. The Jaumann rate update is approximated as: 𝑛+1 = 𝜎𝑖𝑗 𝜎𝑖𝑗 𝑛 + 𝜎𝑖𝑝 𝑛 Δ𝜔𝑝𝑗 + 𝜎𝑗𝑝 𝑛 Δ𝜔𝑝𝑖, (13.39) where the superscripts on the stress refer to the updated (𝑛 + 1) and reference (𝑛) configurations. The Jaumann rate update of the stress tensor is applied in the global configuration before the constitutive evaluation is performed. In the Hughes-Liu shell the stresses and history variables are stored in the global coordinate system. 13.3.2 Stress Update To evaluate the constitutive relation, the stresses and strain increments are rotated from the global to the lamina coordinate system using the transformation defined previously in Equation (13.35), viz. 𝑙𝑛+1 𝜎𝑖𝑗 = 𝑞𝑖𝑘𝜎𝑘𝑛 𝑛+1𝑞𝑗𝑛, 𝑙𝑛+1 2⁄ Δ𝜀𝑖𝑗 𝑛+1 = 𝑞𝑖𝑘Δ𝜀𝑘𝑛 2⁄ 𝑞𝑗𝑛, (13.40) (13.41) Hughes-Liu Shell LS-DYNA Theory Manual where the superscript 𝑙 indicates components in the lamina (local) coordinate system. The stress is updated incrementally: 𝑙𝑛+1 𝜎𝑖𝑗 𝑙𝑛+1 = 𝜎𝑖𝑗 𝑙𝑛+1 2⁄ + Δ𝜎𝑖𝑗 , and rotated back to the global system: 𝑙𝑛+1 𝑛+1 = 𝑞𝑘𝑖𝜎𝑘𝑛 𝜎𝑖𝑗 𝑞𝑛𝑗, before computing the internal force vector. 13.3.3 Incremental Strain-Displacement Relations The global stresses are now used to update the internal force vector int = ∫ 𝐓𝑎 𝐟𝑎 T𝐁𝑎 T𝛔𝑑𝜐, (13.42) (13.43) (13.44) int are the internal forces at node 𝑎, 𝐁𝑎 is the strain-displacement matrix in the where 𝐟𝑎 lamina coordinate system associated with the displacements at node 𝑎, and 𝐓𝑎 is the transformation matrix relating the global and lamina components of the strain- displacement matrix. Because the B matrix relates six strain components to twenty-four displacements (six degrees of freedom at four nodes), it is convenient to partition the B matrix into four groups of six: Each 𝐁𝑎 submatrix is further partitioned into a portion due to strain and spin: 𝐁 = [𝐁1 𝐁2 𝐁3 𝐁4], 𝐁𝑎 = [ 𝐁𝑎 𝜔], 𝐁𝑎 𝜀 = 𝐁𝑎 𝐵1 ⎡ 𝐵2 ⎢ ⎢ 𝐵̅̅̅̅2 𝐵̅̅̅̅1 ⎢ ⎢ ⎢ 𝐵̅̅̅̅3 ⎣ 𝐵̅̅̅̅3 𝐵̅̅̅̅2 𝐵4 𝐵5 𝐵̅̅̅̅5 𝐵̅̅̅̅4 𝐵̅̅̅̅1 𝐵̅̅̅̅6 ⎤ ⎥ ⎥ , ⎥ ⎥ 𝐵̅̅̅̅6 𝐵̅̅̅̅5 ⎥ 𝐵̅̅̅̅4⎦ 𝜔 = 𝐁𝑎 where 𝐵̅̅̅̅2 −𝐵̅̅̅̅1 ⎡ ⎢⎢ −𝐵̅̅̅̅3 ⎣ 𝐵̅̅̅̅3 −𝐵̅̅̅̅2 𝐵̅̅̅̅5 −𝐵̅̅̅̅4 𝐵̅̅̅̅1 −𝐵̅̅̅̅6 ⎤ 𝐵̅̅̅̅6 −𝐵̅̅̅̅5 , ⎥⎥ 𝐵̅̅̅̅4 ⎦ 𝐵𝑖 = ⎧ {{{ ⎨ {{{ ⎩ 𝑁𝑎,𝑖 = (𝑁𝑎𝑧𝑎),𝑖−3 = ∂𝑁𝑎 ∂𝑦𝑖 ∂(𝑁𝑎𝑧𝑎) ∂𝑦𝑖−3 for 𝑖 = 1, 2, 3 . for 𝑖 = 4, 5, 6 (13.45) (13.46) (13.47) (13.48) (13.49) Notes on strain-displacement relations: LS-DYNA Theory Manual Hughes-Liu Shell • The derivatives of the shape functions are taken with respect to the lamina coordinate system, e.g.,𝑦 = 𝑞𝑦. • The superscript bar indicates the 𝐵’s are evaluated at the center of the lamina (0, 0, 𝜁 ). The strain-displacement matrix uses the ‘B-Bar’ (𝐵̅̅̅̅)approach advocated by Hughes [1980]. In the NIKE3D and DYNA3D implementations, this entails replacing certain rows of the B matrix and the strain increments with their coun- terparts evaluated at the center of the element. In particular, the strain- displacement matrix is modified to produce constant shear and spin increments throughout the lamina. • The resulting B-matrix is a 8 × 24 matrix. Although there are six strain and three rotations increments, the B matrix has been modified to account for the fact that 𝜎33 will be zero in the integration of Equation (13.44). 13.4 Element Mass Matrix Hughes, Liu, and Levit [Hughes et al., 1981] describe the procedure used to form the shell element mass matrix in problems involving explicit transient dynamics. Their procedure, which scales the rotary mass terms, is used for all shell elements in LS- DYNA including those formulated by Belytschko and his co-workers. This scaling permits large critical time step sizes without loss of stability. The consistent mass matrix is defined by 𝐌 = ∫ 𝜌𝐍T𝐍 𝑑𝜐𝑚 𝜐𝑚 , (13.50) but cannot be used effectively in explicit calculations where matrix inversions are not feasible. In LS-DYNA only three and four-node shell elements are used with linear interpolation functions; consequently, we compute the translational masses from the consistent mass matrix by row summing, leading to the following mass at element node a: 𝑀disp𝑎 = ∫ 𝜌𝜙𝑎 𝑑𝜐 . (13.51) The rotational masses are computed by scaling the translational mass at the node by the factor 𝛼: 𝑀rot𝑎 = ∝ 𝑀disp𝑎, ∝ = max{∝1, ∝2}, ∝1= ⟨𝑧𝑎⟩2 + 12 [𝑧𝑎]2, ∝2= 8ℎ , (13.52) (13.53) (13.54) (13.55) Hughes-Liu Shell LS-DYNA Theory Manual ⟨𝑧𝑎⟩ = (𝑧𝑎 + + 𝑧𝑎 −) , [𝑧𝑎] = 𝑧𝑎 −. + − 𝑧𝑎 (13.56) (13.57) 13.5 Accounting for Thickness Changes Hughes and Carnoy [1981] describe the procedure used to update the shell thickness due to large membrane stretching. Their procedure with any necessary modifications is used across all shell element types in LS-DYNA. One key to updating the thickness is an accurate calculation of the normal strain component Δ𝜀33. This strain component is easily obtained for elastic materials but can require an iterative algorithm for nonlinear material behavior. In LS-DYNA we therefore default to an iterative plasticity update to accurately determine Δ𝜀33. Hughes and Carnoy integrate the strain tensor through the thickness of the shell in order to determine a mean value Δ𝜀̅𝑖𝑗: Δ𝜀̅𝑖𝑗 = ∫ Δ𝜀𝑖𝑗 −1 𝑑𝜁 , and then project it to determine the straining in the fiber direction: 𝛆̅ 𝑓 = 𝐘̂TΔ𝛆̅𝐘̂. (13.58) (13.59) Using the interpolation functions through the integration points the strains in the fiber directions are extrapolated to the nodal points if 2 × 2 selectively reduced integration is employed. The nodal fiber lengths can now be updated: 𝑛+1 = ℎ𝑎 ℎ𝑎 𝑛 (1 + 𝜀̅𝑎 𝑓 ). (13.60) 13.6 Fully Integrated Hughes-Liu Shells It is well known that one-point integration results in zero energy modes that must be resisted. The four-node under integrated shell with six degrees of freedom per node has nine zero energy modes, six rigid body modes, and four unconstrained drilling degrees of freedom. Deformations in the zero energy modes are always troublesome but usually not a serious problem except in regions where boundary conditions such as point loads are active. In areas where the zero energy modes are a problem, it is highly desirable to provide the option of using the original formulation of Hughes-Liu with selectively reduced integration. LS-DYNA Theory Manual Hughes-Liu Shell Figure 13.5. Selectively reduced integration rule results in four inplane points being used. The major disadvantages of full integration are two-fold: nearly four times as much data must be stored; the operation count increases three- to fourfold. The level 3 loop is added as shown in Figure 13.6 1. 2. However, these disadvantages can be more than offset by the increased reliability and accuracy. We have implemented two version of the Hughes-Liu shell with selectively reduced integration. The first closely follows the intent of the original paper, and therefore no assumptions are made to reduce costs, which are outlined in operation counts in Table 10.1. These operation counts can be compared with those in Table 10.2 for the Hughes-Liu shell with uniformly reduced integration. The second formulation, which reduces the number of operation by more than a factor of two, is referred to as the co-rotational Hughes-Liu shell in the LS-DYNA user’s manual. This shell is considerably cheaper due to the following simplifications: • Strains rates are not centered. The strain displacement matrix is only computed at time 𝑛 + 1 and not at time 𝑛 + 1 ⁄ 2. • The stresses are stored in the local shell system following the Belytschko-Tsay shell. The transformations of the stresses between the local and global coordi- nate systems are thus avoided. • The Jaumann rate rotation is not performed, thereby avoiding even more computations. This does not necessarily preclude the use of the shell in large deformations. • To study the effects of these simplifying assumptions, we can compare results with those obtained with the full Hughes-Liu shell. Thus far, we have been able to get comparable results. Hughes-Liu Shell LS-DYNA Theory Manual LEVEL L1 - Do over each element group gather data, midstep geometry calculation LEVEL 2 - For each thickness integration point center of element calculations for selective reduced integration LEVEL 3 - Do over 4 Gauss points stress update and force contributions LEVEL 2 - Completion LEVEL L1 - Completion Figure 13.6. An inner loop, LEVEL 3, is added for the Hughes-Liu shell with selectively reduced integration. LEVEL L1 - Once per element Midstep translation geometry, etc. Midstep calculation of 𝑌̂ 318 204 LEVEL L2 - For each integration point through thickness (NT points) Strain increment at (0, 0, 𝜁 ) 316 Hughes-Winget rotation matrix 33 Square root of Hughes-Winget matrix Rotate strain increments into lamina coordinates Calculate rows 3-8 of B matrix 919 47 66 LEVEL L3 - For each integration point in lamina Rotate stress to n+1/2 configuration 75 Incremental displacement gradient matrix Rotate stress to lamina system Rotate strain increments to lamina system Constitutive model model dependent Rotate stress back to global system Rotate stress to n+1 configuration 75 Calculate rows 1 and 2 of B matrix Stresses in n+1 lamina system Stress divergence 245 75 75 69 358 370 55 LS-DYNA Theory Manual Hughes-Liu Shell TOTAL 522 +NT {1381 +4 * 1397} Table 10.1. Operation counts for the Hughes-Liu shell with selectively reduced integration. LEVEL L1 - Once per element Calculate displacement increments Element areas for time step Calculate 𝑌̂ 238 53 24 LEVEL L2 and L3 - Integration point through thickness (NT points) 284 Incremental displacement gradient matrix Jaumann rotation for stress 33 Rotate stress into lamina coordinates Rotate stain increments into lamina coordinates Constitutive model model dependent Rotate stress to n+1 global coordinates 69 125 Stress divergence 75 81 LEVEL L1 - Cleanup Finish stress divergence Hourglass control 356 60 TOTAL 731 +NT * 667 Table 10.2. Operation counts for the LS-DYNA implementation of the uniformly reduced Hughes-Liu shell. LS-DYNA Theory Manual Transverse Shear Treatment For Layered Shell 14 Transverse Shear Treatment For Layered Shell The shell element formulations that include the transverse shear strain components are based on the first order shear deformation theory, which yield constant through thickness transverse shear strains. This violates the condition of zero traction on the top and bottom surfaces of the shell. Normally, this is corrected by the use of a shear correction factor. The shear correction factor is 5/6 for isotropic materials; however, this value is incorrect for sandwich and laminated shells. Not accounting for the correct transverse shear strain and stress could yield a very stiff behavior in sandwich and laminated shells. This problem is addressed here by the use of the equilibrium equations without gradient in the y-direction as described by what follows. Consider the stresses in a layered shell: (𝑖)(𝜀𝑥 (𝑖) = 𝐶11 𝜎𝑥 (𝑖)𝜀𝑥 (𝑖) = 𝐶12 𝜎𝑦 (𝑖)(𝜀𝑥𝑦 (𝑖) = 𝐶44 𝜏𝑥𝑦 ∘ + 𝑧𝜒𝑥) + 𝐶12 (𝑖)𝜀𝑦 ∘ + 𝐶22 ∘ + 𝑧(𝐶12 ∘ + 𝑧𝜒𝑥𝑦). (𝑖)(𝜀𝑦 (𝑖)𝜒𝑥 + 𝐶22 ∘ + 𝑧𝜒𝑦) = 𝐶11 (𝑖)𝜒𝑦, (𝑖)𝜀𝑥 ∘ + 𝐶12 (𝑖)𝜀𝑦 ∘ + 𝑧(𝐶11 (𝑖)𝜒𝑥 + 𝐶12 (𝑖)𝜒𝑦), Assume that the bending center 𝑧̅𝑥 is known. Then (𝑖)𝜒𝑦) + 𝐶11 (𝑖) = (𝑧 − 𝑧̅𝑥)(𝐶11 𝜎𝑥 (𝑖)𝜒𝜒 + 𝐶12 (𝑖)𝜀𝑥(𝑧̅𝑥) + 𝐶12 (𝑖)𝜀𝑦(𝑧̅𝑥). The bending moment is given by the following equation: 𝑁𝐿 ⎜⎛∑ 𝐶11 ⎝ 𝑖=1 𝑧𝑖 𝑧𝑖−1 (𝑖) ∫ (𝑧 − 𝑧̅𝑥)2 𝑀𝑥𝑥 = 𝜒𝑥 or 𝑁𝐿 𝑑𝑧 ⎟⎞ + 𝜒𝑦 ⎠ ⎜⎛∑ 𝐶12 ⎝ 𝑖=1 𝑧𝑖 𝑧𝑖−1 (𝑖) ∫ (𝑧 − 𝑧̅𝑥)2 𝑑𝑧 ⎟⎞ ⎠ 𝑀𝑥𝑥 = 𝑁𝐿 [𝜒𝑥 ∑ 𝐶11 (𝑖)[(𝑧𝑖 𝑖=1 3 − 𝑧𝑖−1 3 ) − (𝑧𝑖 − 𝑧𝑖−1)𝑧̅𝑥 2] + 𝜒𝑦 ∑ 𝐶12 (𝑖)[(𝑧𝑖 3 − 𝑧𝑖−1 3 ) − (𝑧𝑖 − 𝑧𝑖−1)𝑧̅𝑥 2] ] 𝑁𝐿 𝑖=1 (14.1) (14.2) (14.3) (14.4) Transverse Shear Treatment For Layered Shell LS-DYNA Theory Manual where “𝑁𝐿” is the number of layers in the material. Assume 𝜀𝑦 = 0 and 𝜎𝑥 = 𝐸𝜒𝜀𝜒, let 𝑁𝐿 (𝐸𝐼)𝑥 = ∑ 𝑖=1 (𝑖)[(𝑧𝑖 𝐸𝑥 3 − 𝑧𝑖−1 3 ) − (𝑧𝑖 − 𝑧𝑖−1)𝑧̅𝑥 2], then and 𝜀𝑥 = 𝑧 − 𝑧̅𝑥 = (𝑧 − 𝑧̅𝑥)𝜒𝑥, 𝑀𝑥𝑥 = (𝜒𝑥(𝐸𝐼)𝑥), 𝜒𝑥 = 3𝑀𝑥𝑥 (𝐸𝐼)𝑥 . Therefore, the stress becomes (𝑖) = 𝜎𝑥 3𝑀𝑥𝑥𝐸𝑥 (𝑖)(𝑧 − 𝑧̅𝑥) (𝐸𝐼)𝑥 . Now considering the first equilibrium equation, one can write the following: ∂𝜏𝑥𝑧 ∂𝑧 = − ∂𝜎𝑥 ∂𝑥 = − 3𝑄𝑥𝑧𝐸𝑥 (𝑗)(𝑧 − 𝑧̅𝑥) , (𝐸𝐼)𝑥 (𝑗) = − 𝜏𝑥𝑧 3𝑄𝑥𝑧𝐸𝑥 (𝑗) (𝑧2 (𝐸𝐼)𝑥 − 𝑧𝑧̅𝑥) + 𝐶𝑗, (14.5) (14.6) (14.7) (14.8) (14.9) (14.10) (14.11) where 𝑄𝑥𝑧 is the shear force and 𝐶𝑗 is the constant of integration. This constant is obtained from the transverse shear stress continuity requirement at the interface of each layer. Let then 𝑄𝑥𝑧𝐸𝑥 (𝑖) ( 𝑧𝑖−1 − 𝑧𝑖−1𝑧̅𝑥) (𝐸𝐼)𝑥 𝐶𝑗 = + 𝜏𝑥𝑧 𝑖−1, and (𝑖) = 𝜏𝑥𝑧 𝜏𝑥𝑧 (𝑖−1) + (𝑖) 𝑄𝑥𝑧𝐸𝑥 (𝐸𝐼)𝑥 𝑧𝑖−1 [ − 𝑧𝑖−1𝑧̅𝑥 − 𝑧2 + 𝑧𝑧̅𝑥]. For the first layer (14.12) (14.13) LS-DYNA Theory Manual Transverse Shear Treatment For Layered Shell 𝜏𝑥𝑧 = − (1) 3𝑄𝑥𝑧𝐶11 (𝐸𝐼)𝑥 𝑧2 − 𝑧𝑜 [ − 𝑧̅𝑥(𝑧 − 𝑧𝑜)], (14.14) for subsequent layers 𝜏𝑥𝑧 = 𝜏𝑥𝑧 (𝑖−1) − (𝑖) 3𝑄𝑥𝑧𝐶11 (𝐸𝐼)𝑥 𝑧2 − 𝑧𝑖−1 [ − 𝑧̅𝑥(𝑧 − 𝑧𝑖−1)] , 𝑧𝑖−1 ≤ 𝑧 ≤ 𝑧𝑖. (14.15) (𝑖−1) is the stress in previous layer at the interface with the current layer. The Here 𝜏𝑥𝑧 shear stress can also be expressed as follows: 𝜏𝑥𝑧 = − (𝑖) 3𝑄𝑥𝑧𝐶11 (𝐸𝐼)𝑥 (𝑖) + [𝑓𝑥 𝑧2 − 𝑧𝑖−1 − 𝑧̅𝑥(𝑧 − 𝑧𝑖−1)], (14.16) where and (𝑖) = 𝑓𝑥 𝑖−1 (𝑖) ∑ 𝐶11 𝐶11 𝑗=1 (𝑗)ℎ𝑗 [ 𝑧𝑗 + 𝑧𝑗+1 − 𝑧̅𝑥] , ℎ𝑗 = 𝑧𝑗 − 𝑧𝑗−1. (14.17) (14.18) To find 𝑄𝑥𝑧, the shear force, assume that the strain energy expressed through average shear modules, 𝐶̅66, is equal to the strain energy expressed through the derived expressions as follows: 𝑈 = 𝑄𝑥𝑧 𝐶̅66ℎ = ∫ 𝜏𝑥𝑧 𝐶66 𝑑𝑧, 2 ∫ 𝐶11 𝐶66 (𝑖) + [𝑓𝑥 2 ) (𝑧2 − 𝑧𝑖−1 − 𝑧̅𝑥(𝑧 − 𝑧𝑖−1)] 𝑑𝑧 9ℎ (𝐸𝐼)𝑥 9ℎ (𝐸𝐼)𝑥 60 𝐶̅66 = = = then 9ℎ (𝑖) + 𝑁𝐿 2 ∑ 𝑖=1 [𝑓𝑥 𝑧𝑖 ∫ 𝑧𝑖−1 (𝑖))2 (𝐶11 (𝑖) 𝐶66 (𝑖))2ℎ (𝐶11 𝐶66 + 𝑧̅𝑥ℎ𝑖[20𝑧̅𝑥ℎ𝑖 + 35𝑧𝑖−1 2 ) + 8𝑧𝑖−1 − 7𝑧𝑖−1 𝑁𝐿 2 ∑ 𝑖[60𝑓𝑥 4 }, {𝑓𝑥 (𝐸𝐼)𝑥 𝑧2 − 𝑧𝑖−1 − 𝑧̅𝑥(𝑧 − 𝑧𝑖−1)] 𝑑𝑧 𝑖 + 20ℎ𝑖(𝑧𝑖 + 2𝑧𝑖−1 − 3𝑧̅𝑥)] 2 − 10𝑧𝑖−1(𝑧𝑖 + 𝑧𝑖−1) − 15𝑧𝑖 2] + 𝑧𝑖(𝑧𝑖 + 𝑧𝑖−1)(3𝑧𝑖 𝑄𝑥𝑧 = 𝜏̅𝑥𝑧ℎ = 𝐶̅66𝛾̅̅̅̅𝑥𝑧ℎ, to calculate 𝑧̅𝑥 use 𝜏𝑥𝑧 for last layer at surface 𝑧 = 0, 𝑁𝐿 (𝑖) ∑ 𝐶11 𝑖=1 [( 2 − 𝑧𝑖−1 𝑧𝑖 ) − 𝑧̅𝑥(𝑧𝑖 − 𝑧𝑖−1)] = 0, (14.19) (14.20) (14.21) (14.22) Transverse Shear Treatment For Layered Shell LS-DYNA Theory Manual where Algorithm: 𝑧̅𝑥 = 𝑁𝐿 ∑ 𝐶11 𝑖=1 (𝑖)ℎ𝑖(𝑧𝑖 + 𝑧𝑖+1) . 𝑁𝐿 (𝑖)ℎ𝑖 2 ∑ 𝐶11 𝑖=1 (14.23) The following algorithm is used in the implementation of the transverse shear treatment. 1. Calculate 𝑧̅𝑥 according to equation (14.23) 2. Calculate 𝑓𝑥 𝑖 according to equation (14.17) 3. Calculate 1 𝑁𝐿 (𝑖) 3 ∑ 𝐶11 𝑖=1 (𝑧𝑖 3 − 𝑧𝑖−1 3 ) 4. Calculate ℎ[1 𝑁𝐿 (𝑖) 3 ∑ 𝐶11 𝑖=1 3 − 𝑧𝑖−1 3 )] (𝑧𝑖 5. Calculate 𝐶̅66 according to equation (14.20) 6. Calculate 𝑄𝑥𝑧 = 𝐶̅66𝛾̅̅̅̅𝑥𝑧ℎ 7. Calculate 𝜏𝑥𝑧 according to equation (14.16) Steps 1-5 are performed at the initialization stage. Step 6 is performed in the shell formulation subroutine, and step 7 is performed in the stress calculation inside the constitutive subroutine. LS-DYNA Theory Manual Eight-Node Solid Shell Element 15 Eight-Node Solid Shell Element The isoparametric eight-node brick element discussed in Section 3 forms the basis for tshell formulation 1, a solid shell element with enhancements based on the Hughes-Liu and the Belytschko-Lin-Tsay shells. Like the eight-node brick, the geometry is interpolated from the nodal point coordinates as: 𝑥𝑖(𝑋𝛼, 𝑡) = 𝑥𝑖(𝑋𝛼(𝜉 , 𝜂, 𝜁 ), 𝑡) = ∑ 𝜙𝑗 𝑗=1 (𝜉 , 𝜂, 𝜁 )𝑥𝑖 𝑗(𝑡), 𝜙𝑗 = (1 + 𝜉 𝜉𝑗)(1 + 𝜂𝜂𝑗)(1 + 𝜁 𝜁𝑗). As with solid elements, 𝐍 is the 3 × 24 rectangular interpolation matrix: 𝐍(𝜉 , 𝜂, 𝜁 ) = 𝜑1 ⎡ ⎢ ⎣ 𝜑1 𝜑1 𝜑2 0 … 0 𝜑2 … 𝜑8 0 … 0 ⎤ , ⎥ 𝜑8⎦ 𝛔 is the stress vector: and 𝐁 is the 6 × 24 strain-displacement matrix: 𝛔T = (𝜎𝑥𝑥, 𝜎𝑦𝑦, 𝜎𝑧𝑧, 𝜎𝑥𝑦, 𝜎𝑦𝑧, 𝜎𝑧𝑥), (15.1) (15.2) (15.3) (15.4) Eight-Node Solid Shell Element LS-DYNA Theory Manual Upper shell surface. The numbering of the solid shell determines its orientation Node -1 -1 -1 -1 -1 -1 -1 -1 -1 -1 -1 -1 Figure 15.1. Eight node solid shell element 𝐁 = ∂ ∂𝑥 ⎡ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎣ ∂ ∂𝑦 ∂ ∂𝑧 ∂ ∂𝑦 ∂ ∂𝑥 ∂ ∂𝑧 ∂ ∂𝑧 ⎤ ⎥ ⎥ ⎥ ⎥ ⎥ ⎥ ⎥ ⎥ ⎥ ⎥ ⎥ ⎥ ∂ ⎥ ⎥ ∂𝑦 ⎥ ∂ ⎥ ∂𝑥⎦ 𝐍, (15.5) Terms in the strain-displacement matrix are readily calculated. Note that ∂𝜑𝑖 ∂𝜉 ∂𝜑𝑖 ∂𝜂 ∂𝜑𝑖 ∂𝜁 = = = ∂𝜑𝑖 ∂𝑥 ∂𝜑𝑖 ∂𝑥 ∂𝜑𝑖 ∂𝑥 ∂𝑥 ∂𝜉 ∂𝑥 ∂𝜂 ∂𝑥 ∂𝜁 + + + ∂𝜑𝑖 ∂𝑦 ∂𝜑𝑖 ∂𝑦 ∂𝜑𝑖 ∂𝑦 ∂𝑦 ∂𝜉 ∂𝑦 ∂𝜂 ∂𝑦 ∂𝜁 + + + ∂𝜑𝑖 ∂𝑧 ∂𝜑𝑖 ∂𝑧 ∂𝜑𝑖 ∂𝑧 ∂𝑧 ∂𝜉 ∂𝑧 ∂𝜂 ∂𝑧 ∂𝜁 , , , (15.6) which can be rewritten as LS-DYNA Theory Manual Eight-Node Solid Shell Element ∂𝜑𝑖 ⎤ ⎡ ∂𝜉 ⎥ ⎢ ⎥ ⎢ ∂𝜑𝑖 ⎥ ⎢ ⎥ ⎢ ∂𝜂 ⎥ ⎢ ⎥ ⎢ ∂𝜑𝑖 ⎥ ⎢ ∂𝜁 ⎦ ⎣ = ∂𝑥 ∂𝜉 ∂𝑥 ∂𝜂 ∂𝑥 ∂𝜁 ⎡ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎣ ∂𝑦 ∂𝜉 ∂𝑦 ∂𝜂 ∂𝑦 ∂𝜁 ∂𝑧 ⎤ ∂𝜉 ⎥ ⎥ ∂𝑧 ⎥ ⎥ ∂𝜂 ⎥ ⎥ ∂𝑧 ⎥ ∂𝜁 ⎦ ∂𝜑𝑖 ⎤ ⎡ ∂𝑥 ⎥ ⎢ ⎥ ⎢ ∂𝜑𝑖 ⎥ ⎢ ⎥ ⎢ ∂𝑦 ⎥ ⎢ ∂𝜑𝑖 ⎥ ⎢ ∂𝑧 ⎦ ⎣ = 𝐉 ∂𝜑𝑖 ⎤ ∂𝑥 ⎥ ⎥ ∂𝜑𝑖 ⎥ . ⎥ ∂𝑦 ⎥ ∂𝜑𝑖 ⎥ ∂𝑧 ⎦ ⎡ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎣ Inverting the Jacobian matrix, 𝐉, we can solve for the desired terms ∂𝜑𝑖 ⎤ ⎡ ∂𝑥 ⎥ ⎢ ⎥ ⎢ ∂𝜑𝑖 ⎥ ⎢ ⎥ ⎢ ∂𝑦 ⎥ ⎢ ∂𝜑𝑖 ⎥ ⎢ ∂𝑧 ⎦ ⎣ = 𝐉−1 ∂𝜑𝑖 ⎤ ⎡ ∂𝜉 ⎥ ⎢ ⎥ ⎢ ∂𝜑𝑖 ⎥ ⎢ ⎥ ⎢ ∂𝜂 ⎥ ⎢ ⎥ ⎢ ∂𝜑𝑖 ⎥ ⎢ ∂𝜁 ⎦ ⎣ . (15.7) (15.8) To obtain shell-like behavior from the solid element, it is necessary to use multiple integration points through the shell thickness along the 𝜁 axis while employing a plane stress constitutive subroutine. Consequently, it is necessary to construct a reference surface within the brick shell. We locate the reference surface midway between the upper and lower surfaces and construct a local coordinate system exactly as was done for the Belytschko-Lin-Tsay shell element. Following the procedure outlined in Section 7, Equations (7.1) – (7.3), the local coordinate system can be constructed as depicted in Figure 15.2. Equation (7.5a) gives the transformation matrix in terms of the local basis: {𝐀} = {⎧𝐴𝑥 }⎫ 𝐴𝑦 𝐴𝑧⎭}⎬ ⎩{⎨ = 𝑒3𝑥 𝑒1𝑥 𝑒2𝑥 ⎥⎤ ⎢⎡ 𝑒1𝑦 𝑒2𝑦 𝑒3𝑦 𝑒3𝑧 ⎦ 𝑒1𝑧 𝑒2𝑧 ⎣ ⎧𝐴̂𝑥 ⎫ }} {{ 𝐴̂𝑦 ⎬ ⎨ }} {{ 𝐴̂𝑧⎭ ⎩ = [𝛍]{𝐀̂} = [𝐪]T{𝐀̂}. (15.9) As with the Hughes-Liu shell, the next step is to perform the Jaumann rate update: 𝑛+1 = 𝜎𝑖𝑗 𝜎𝑖𝑗 𝑛 + 𝜎𝑖𝑝 𝑛 Δ𝜔𝑝𝑗 + 𝜎𝑗𝑝 𝑛 Δ𝜔𝑝𝑖, (15.10) to account for the material rotation between time steps 𝑛 and 𝑛 + 1. The Jaumann rate update of the stress tensor is applied in the global configuration before the constitutive evaluation is performed. In the solid shell, as in the Hughes-Liu shell, the stresses and history variables are stored in the global coordinate system. To evaluate the constitutive relation, the stresses and the strain increments are rotated from the global to the lamina coordinate system using the transformation defined previously: 𝑙𝑛+1 𝜎𝑖𝑗 = 𝑞𝑖𝑘𝜎𝑘𝑛 𝑛+1𝑞𝑗𝑛, 𝑙𝑛+1 2⁄ Δ𝜀𝑖𝑗 𝑛+1 = 𝑞𝑖𝑘Δ𝜀𝑘𝑛 2⁄ 𝑞𝑗𝑛, (15.11) (15.12) Eight-Node Solid Shell Element LS-DYNA Theory Manual A reference surface is constructed within the solid shell element and the local reference system is defined. y^ e^ s3 e^ r42 r31 e^ s1 x^ r21 Figure 15.2. Construction of the reference surface in the solid shell element. where the superscript l indicates components in the lamina (local) coordinate system. The stress is updated incrementally: 𝑙𝑛+1 𝜎𝑖𝑗 𝑙𝑛+1 = 𝜎𝑖𝑗 𝑙𝑛+1 2⁄ + Δ𝜎𝑖𝑗 . Independently from the constitutive evaluation 𝑙 = 0, 𝜎33 (15.13) (15.14) which ensures that the plane stress condition is satisfied, we update the normal stress which is used as a penalty to maintain the thickness of the shell: penalty) (𝜎33 n+1 = (𝜎33 penalty) + 𝐸Δ𝜀33 , (15.15) where 𝐸 is the elastic Young’s modulus for the material. The stress tensor of Equation (15.13) is rotated back to the global system: 𝑙 ) 𝑛+1 = 𝑞𝑘𝑖(𝜎𝑘𝑛 𝜎𝑖𝑗 𝑛+1 𝑞𝑛𝑗. (15.16) A penalty stress tensor is then formed by transforming the normal penalty stress tensor (a null tensor except for the 33 term) back to the global system: n+1 penalty) (𝜎𝑖𝑗 = 𝑞𝑘𝑖 [(𝜎𝑖𝑗 penalty) 𝑛+1 ] 𝑞𝑛𝑗, 15-4 (Eight-Node Solid Shell Element) LS-DYNA Theory Manual Eight-Node Solid Shell Element before computing the internal force vector. The internal force vector can now be computed: 𝐟int = ∫(𝐁𝑛+1) [𝝈𝑛+1 + (𝝈penalty) 𝑛+1 ] 𝑑𝜐. (15.18) The brick shell exhibits no discernible locking problems with this approach. The treatment of the hourglass modes is identical to that described for the solid elements in Section 3. LS-DYNA Theory Manual Eight-Node Solid Element for Thick Shell Simulations 16 Eight-Node Solid Element for Thick Shell Simulations 16.1 Abstract Tshell formulation 3 is an eight-node hexahedral element incorporated into LS- DYNA to simulate thick shell structures. The element formulation is derived in a co- rotational coordinate system and the strain operator is calculated with a Taylor series expansion about the center of the element. Special treatments are made on the dilatational strain component and shear strain components to eliminate the volumetric and shear locking. The use of consistent tangential stiffness and geometric stiffness greatly improves the convergence rate in implicit analysis. 16.2 Introduction Large-scale finite element analyses are extensively used in engineering designs and process controls. For example, in automobile crashworthiness, hundreds of thousands of unknowns are involved in the computer simulation models, and in metal forming processing, tests in the design of new dies or new products are done by numerical computations instead of costly experiments. The efficiency of the elements is of crucial importance to speed up the design processes and reduce the computational costs for these problems. Over the past ten years, considerable progress has been achieved in developing fast and reliable elements. In the simulation of shell structures, Belytschko-Lin-Tsay [Belytschko, 1984a] and Hughes-Liu [Hughes, 1981a and 1981b] shell elements are widely used. However, in some cases thick shell elements are more suitable. For example, in the sheet metal forming with large curvature, traditional thin shell elements cannot give satisfactory Eight-Node Solid Element for Thick Shell Simulations LS-DYNA Theory Manual results. Also thin shell elements cannot give us detailed strain information though the thickness. In LS-DYNA, the eight-node solid thick shell element is still based on the Hughes-Liu and Belytschko-Lin-Tsay shells [Hallquist, 1998]. A new eight-node solid element based on Liu, 1985, 1994 and 1998 is incorporated into LS-DYNA, intended for thick shell simulation. The strain operator of this element is derived from a Taylor series expansion and special treatments on strain components are utilized to avoid volumetric and shear locking. The organization of this paper is as follows. The element formulations are described in the next section. Several numerical problems are studied in the third section, followed by the conclusions. 16.3 Element Formulations 16.3.1 Strain Operator The new element is based on the eight-node hexahedral element proposed and enhanced by Liu, 1985, 1994, 1998. For an eight-node hexahedral element, the spatial coordinates, 𝑥𝑖, and the velocity components, 𝑣𝑖, in the element are approximated in terms of nodal values, x𝑖aand v𝑖a, by 𝑥𝑖 = ∑ 𝑁𝑎 𝑎=1 (𝜉 , 𝜂, 𝜁 )𝑥𝑖𝑎, (16.1) 𝑣𝑖 = ∑ 𝑁𝑎 𝑎 = 1 (𝜉 , 𝜂, 𝜁 )𝑣𝑖𝑎, 𝑖 = 1, 2, 3, 𝑁𝑎(𝜉, 𝜂, 𝜁 ) = (1 + 𝜉𝑎𝜉 )(1 + 𝜂𝑎𝜂)(1 + 𝜁𝑎𝜁 ), (16.2) (16.3) and the subscripts 𝑖 and a denote coordinate components ranging from one to three and the element nodal numbers ranging from one to eight, respectively. The referential coordinates 𝜉 , 𝜂, and 𝜁 of node a are denoted by 𝜉𝑎, 𝜂𝑎, and 𝜁𝑎, respectively. The strain rate (or rate of deformation), 𝛆̇, is composed of six components, and is related to the nodal velocities by a strain operator, 𝐁̅̅̅̅̅, 𝛆̇T = [𝜀𝑥𝑥 𝜀𝑦𝑦 𝜀𝑧𝑧 𝜀𝑥𝑦 𝜀𝑦𝑧 𝜀𝑧𝑥], 𝛆̇ = 𝐁̅̅̅̅̅(𝜉 , 𝜂, 𝜁 )𝐯, where 𝐯T = [vx1 vy1 vz1 ⋯ vx8 vy8 vz8], (16.4) (16.5) (16.6) LS-DYNA Theory Manual Eight-Node Solid Element for Thick Shell Simulations 𝐁̅̅̅̅̅ = B̅̅̅̅̅𝑥𝑥 ⎤ ⎡ B̅̅̅̅̅𝑦𝑦 ⎥ ⎢ ⎥ ⎢ B̅̅̅̅̅𝑧𝑧 ⎥ ⎢ ⎥ ⎢ B̅̅̅̅̅𝑥𝑦 ⎥ ⎢ ⎥ ⎢ ⎥ ⎢ B̅̅̅̅̅𝑦𝑧 ⎥ ⎢ B̅̅̅̅̅𝑧𝑥⎦ ⎣ = ⎡ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎣ 𝐵1(1) 𝐵2(1) ⋯ 𝐵1(8) ⋯ 𝐵3(1) ⋯ 𝐵2(1) 𝐵1(1) ⋯ 𝐵2(8) 𝐵1(8) 𝐵2(8) ⎤ ⎥ ⎥ 𝐵3(8) ⎥ , ⎥ ⎥ 𝐵3(8) 𝐵2(8) ⎥ 𝐵1(8)⎦ 𝐵3(1) 𝐵3(1) 𝐵2(1) ⋯ 𝐵1(1) ⋯ 𝐵3(8) B1 ⎤ = ⎡ B2 ⎥ ⎢ B3⎦ ⎣ 𝑁,𝑥 (𝜉 , 𝜂, 𝜁 ) ⎤ ⎡ 𝑁,𝑦 (𝜉 , 𝜂, 𝜁 ) . ⎥⎥ ⎢⎢ 𝑁,𝑧 (𝜉 , 𝜂, 𝜁 )⎦ ⎣ (16.7) (16.8) Unlike standard solid element where the strain operator is computed by differentiating the shape functions, the strain operator for this new element is expanded in a Taylor series about the element center up to bilinear terms as follows [Liu, 1994, 1998], 𝐁̅̅̅̅̅(𝜉 , 𝜂, 𝜁 ) = 𝐁̅̅̅̅̅(0) + 𝐁̅̅̅̅̅,𝜉 (0)𝛏 + 𝐁̅̅̅̅̅,𝜂 (0)𝛈 + 𝐁̅̅̅̅̅,𝜁 (0)𝛇 + 𝐁̅̅̅̅̅,𝜉𝜂 (0)𝛏𝛈 + 𝐁̅̅̅̅̅,𝜂𝜁 (0)𝛈𝛇 + 𝐁̅̅̅̅̅,𝜁𝜉 (0)𝛇𝛏 . Let T = 𝐱T = [𝑥1 𝐱1 𝑥2 𝑥3 𝑥4 𝑥5 𝑥6 𝑥7 𝑥8], T = 𝐲T = [𝑦1 𝐱2 𝑦2 𝑦3 T = 𝐳T = [𝑧1 𝐱3 𝑧2 𝑧3 𝑦4 𝑧4 𝑦5 𝑦6 𝑦7 𝑦8], 𝑧5 𝑧6 𝑧7 𝑧8], 𝛏T = [−1 1 −1 −1 1 −1], 𝛈T = [−1 −1 1 −1 −1 1], 𝛇T = [−1 −1 −1 −1 the Jacobian matrix at the center of the element can be evaluated as 1], 𝐉(0) = [J𝑖𝑗] = 𝛏T𝐲 𝛏T𝐳 𝛏T𝐱 ⎤ ⎡ 𝛈T𝐱 𝛈T𝐲 𝛈T𝐳 ⎥⎥ ⎢⎢ 𝛇T𝐲 𝛇T𝐳⎦ 𝛇T𝐱 ⎣ ; (16.9) (16.10) (16.11) (16.12) (16.13) (16.14) (16.15) (16.16) the determinant of the Jacobian matrix is denoted by j0 and the inverse matrix of 𝐉(0) is denoted by 𝐃 𝐃 = [D𝑖𝑗] = 𝐉−1(0). (16.17) The gradient vectors and their derivatives with respect to the natural coordinates at the center of the element are given as follows, Eight-Node Solid Element for Thick Shell Simulations LS-DYNA Theory Manual 𝐛1 = 𝐍,𝑥 (0) = 𝐛2 = 𝐍,𝑦 (0) = 𝐛3 = 𝐍,𝑧 (0) = [𝐷11𝛏 + 𝐷12𝛈 + 𝐷13𝛇], [𝐷21𝛏 + 𝐷22𝛈 + 𝐷23𝛇], [𝐷31𝛏 + 𝐷32𝛈 + 𝐷33𝛇], 𝐛1,𝜉 = 𝐍,𝑥𝜉 (0) = 𝐛2,𝜉 = 𝐍,𝑦𝜉 (0) = 𝐛3,𝜉 = 𝐍,𝑧𝜉 (0) = 𝐛1,𝜂 = 𝐍,𝑥𝜂 (0) = 𝐛2,𝜂 = 𝐍,𝑦𝜂 (0) = 𝐛3,𝜂 = 𝐍,𝑧𝜂 (0) = 𝐛1,𝜁 = 𝐍,𝑥𝜁 (0) = 𝐛2,𝜁 = 𝐍,𝑦𝜁 (0) = 𝐛3,𝜁 = 𝐍,𝑧𝜁 (0) = [𝐷12𝜸1 + 𝐷13𝛄2], [𝐷22𝛄1 + 𝐷23𝛄2], [𝐷32𝛄1 + 𝐷33𝛄2], [𝐷11𝛄1 + 𝐷13𝛄3], [𝐷21𝛄1 + 𝐷23𝛄3], [𝐷31𝛄1 + 𝐷33𝛄3], [𝐷11𝛄2 + 𝐷12𝛄3], [𝐷21𝛄2 + 𝐷22𝛄3], [𝐷31𝛄2 + 𝐷32𝛄3], 𝐛1,𝜉𝜂 = 𝐍,𝑥𝜉𝜂 (0) = 𝐛2,𝜉𝜂 = 𝐍,𝑦𝜉𝜂 (0) = 𝐛3,𝜉𝜂 = 𝐍,𝑧𝜉𝜂 (0) = 𝐛1,𝜂𝜁 = 𝐍,𝑥𝜂𝜁 (0) = 𝐛2,𝜂𝜁 = 𝐍,𝑦𝜂𝜁 (0) = [𝐷13𝛄4 − (𝐩1 T𝐱𝑖)𝐛𝑖,𝜉 − (𝐫1 T𝐱𝑖)𝐛𝑖,𝜂], [𝐷23𝛄4 − (𝐛2 T𝐱𝑖)𝐛𝑖,𝜉 − (𝐫2 T𝐱𝑖)𝐛𝑖,𝜂], [𝐷33𝛄4 − (𝐩3 T𝐱𝑖)𝐛𝑖,𝜉 − (𝐫3 T𝐱𝑖)𝐛𝑖,𝜂], [𝐷11𝛄4 − (𝐪1 T𝐱𝑖)𝐛𝑖,𝜂 − (𝐩1 T𝐱𝑖)𝐛𝑖,𝜁 ], [𝐷21𝛄4 − (𝐪2 T𝐱𝑖)𝐛𝑖,𝜂 − (𝐩2 T𝐱𝑖)𝐛𝑖,𝜁 ], (16.18) (16.19) (16.20) (16.21) (16.22) (16.23) (16.24) (16.25) (16.26) (16.27) (16.28) (16.29) (16.30) (16.31) (16.32) (16.33) (16.34) LS-DYNA Theory Manual Eight-Node Solid Element for Thick Shell Simulations 𝐛3,𝜂𝜁 = 𝐍,𝑧𝜂𝜁 (0) = 𝐛1,𝜁𝜉 = 𝐍,𝑥𝜁𝜉 (0) = 𝐛2,𝜁𝜉 = 𝐍,𝑦𝜁𝜉 (0) = 𝐛3,𝜁𝜉 = 𝐍,𝑧𝜁𝜉 (0) = [𝐷31𝛄4 − (𝐪3 T𝐱𝑖)𝐛𝑖,𝜂 − (𝐩3 T𝐱𝑖)𝐛𝑖,𝜁 ], [𝐷12𝛄4 − (𝐫1 T𝐱𝑖)𝐛𝑖,𝜁 − (𝐪1 T𝐱𝑖)𝐛𝑖,𝜉 ], [𝐷22𝛄4 − (𝐫2 T𝐱𝑖)𝐛𝑖,𝜁 − (𝐪2 T𝐱𝑖)𝐛𝑖,𝜉 ], [𝐷32𝛄4 − (𝐫3 T𝐱𝑖)𝐛𝑖,𝜁 − (𝐪3 T𝐱𝑖)𝐛𝑖,𝜉 ], where and 𝐩𝑖 = 𝐷𝑖1𝐡1 + 𝐷𝑖3𝐡3, 𝐪𝑖 = 𝐷𝑖1𝐡2 + 𝐷𝑖2𝐡3, 𝐫𝑖 = 𝐷𝑖2𝐡1 + 𝐷𝑖3𝐡2, 𝜸𝛼 = 𝐡𝛼 − (𝐡𝛼 T𝐱𝑖)𝐛𝑖, T = [1 −1 𝐡1 1 −1 1 −1 1 −1], T = [1 −1 −1 𝐡2 1 −1 1 −1], T = [1 𝐡3 1 −1 −1 −1 −1 1], T = [−1 𝐡4 1 −1 1 −1 1 −1]. (16.35) (16.36) (16.37) (16.38) (16.39) (16.40) (16.41) (16.42) (16.43) (16.44) (16.45) (16.46) In the above equations 𝐡1 is the 𝜉𝜂-hourglass vector, 𝐡2 the 𝜂𝜁 -hourglass vector, 𝐡3 the 𝜁𝜉 -hourglass vector and 𝐡4the 𝜉𝜂𝜁 -hourglass vector. They are the zero energy- deformation modes associated with the one-point-quadrature element which result in a non-constant strain field in the element [Flanagan, 1981, Belytschko, 1984 and Liu, 1984]. The 𝛾𝛼 in equations (16.21)–(16.38) are the stabilization vectors. They are orthogonal to the linear displacement field and provide a consistent stabilization for the element. The strain operators, 𝐁̅̅̅̅̅(𝜉 , 𝜂, 𝜁 ), can be decomposed into two parts, the dilatational part, 𝐁̅̅̅̅̅dil(𝜉 , 𝜂, 𝜁 ), and the deviatoric part, 𝐁̅̅̅̅̅dev(𝜉 , 𝜂, 𝜁 ), both of which can be expanded about the element center as in Equation (16.9) 𝐁̅̅̅̅̅dil(𝛏, 𝛈, 𝛇) = 𝐁̅̅̅̅̅dil(0) + 𝐁̅̅̅̅̅,𝜉 +𝐁̅̅̅̅̅,𝜉𝜂 dil(0)𝛏 + 𝐁̅̅̅̅̅,𝜂 dil (0)𝛇𝛏, dil (0)𝛈𝛇 + 𝐁̅̅̅̅̅,𝜁𝜉 dil(0)𝛏𝛈 + 𝐁̅̅̅̅̅,𝜂𝜁 dil(0)𝛈 + 𝐁̅̅̅̅̅,𝜁 dil(0)𝛇 (16.47) Eight-Node Solid Element for Thick Shell Simulations LS-DYNA Theory Manual 𝐁̅̅̅̅̅dev(𝜉 , 𝜂, 𝜁 ) = 𝐁̅̅̅̅̅dev(0) + 𝐁̅̅̅̅̅,𝜉 +𝐁̅̅̅̅̅,𝜉𝜂 dev(0)𝛏𝛈 + 𝐁̅̅̅̅̅,𝜂𝜁 dev(0)𝛈𝛇 + 𝐁̅̅̅̅̅,𝜁𝜉 dev(0)𝜉 + 𝐁̅̅̅̅̅,𝜂 dev(0)𝛇𝛏, dev(0)𝛈 + 𝐁̅̅̅̅̅,𝜁 dev(0)𝛇 (16.48) To avoid volumetric locking, the dilatational part of the strain operators is evaluated only at one quadrature point, the center of the element, i.e., they are constant terms 𝐁̅̅̅̅̅dil(𝝃 , 𝜼, 𝜻) = 𝐁̅̅̅̅̅dil(0). (16.49) To remove shear locking, the deviatoric strain submatrices can be written in an orthogonal co-rotational coordinate system rotating with the element as dev(𝜉 , 𝜂, 𝜁 ) = B̅̅̅̅̅𝑥𝑥 B̅̅̅̅̅𝑥𝑥 +B̅̅̅̅̅𝑥𝑥,𝜉𝜂 dev (0)𝜉𝜂 + B̅̅̅̅̅𝑥𝑥,𝜂𝜁 dev(0) + B̅̅̅̅̅𝑥𝑥,𝜉 dev (0)𝜂𝜁 + B̅̅̅̅̅𝑥𝑥,𝜁𝜉 dev (0)𝜉 + B̅̅̅̅̅𝑥𝑥,𝜂 dev (0)𝜁𝜉 , dev (0)𝜂 + B̅̅̅̅̅𝑥𝑥,𝜁 dev (0)𝜁 dev(𝜉 , 𝜂, 𝜁 ) = B̅̅̅̅̅𝑦𝑦 B̅̅̅̅̅𝑦𝑦 +B̅̅̅̅̅𝑦𝑦,𝜉𝜂 dev (0)𝜉𝜂 + B̅̅̅̅̅𝑦𝑦,𝜂𝜁 dev(0) + B̅̅̅̅̅𝑦𝑦,𝜉 dev (0)𝜂𝜁 + B̅̅̅̅̅𝑦𝑦,𝜁𝜉 dev (0)𝜉 + B̅̅̅̅̅𝑦𝑦,𝜂 dev (0)𝜁𝜉 , dev (0)𝜂 + B̅̅̅̅̅𝑦𝑦,𝜁 dev (0)𝜁 dev(𝜉 , 𝜂, 𝜁 ) = B̅̅̅̅̅𝑧𝑧 B̅̅̅̅̅𝑧𝑧 +B̅̅̅̅̅𝑧𝑧,𝜉𝜂 dev (0)𝜉𝜂 + B̅̅̅̅̅𝑧𝑧,𝜂𝜁 dev(0) + B̅̅̅̅̅𝑧𝑧,𝜉 dev (0)𝜂𝜁 + B̅̅̅̅̅𝑧𝑧,𝜁𝜉 dev(0)𝜉 + B̅̅̅̅̅𝑧𝑧,𝜂 dev (0)𝜁𝜉 , dev(0)𝜂 + B̅̅̅̅̅𝑧𝑧,𝜁 dev(0)𝜁 dev(𝜉 , 𝜂, 𝜁 ) = B̅̅̅̅̅𝑥𝑦 B̅̅̅̅̅𝑥𝑦 dev(0) + B̅̅̅̅̅𝑥𝑦,𝜁 dev (0)𝜁 , dev(𝜉 , 𝜂, 𝜁 ) = B̅̅̅̅̅𝑦𝑧 B̅̅̅̅̅𝑦𝑧 dev(0) + B̅̅̅̅̅𝑦𝑧,𝜉 dev (0)𝜉 , dev(𝜉 , 𝜂, 𝜁 ) = B̅̅̅̅̅𝑧𝑥 B̅̅̅̅̅𝑧𝑥 dev(0) + B̅̅̅̅̅𝑧𝑥,𝜂 dev (0)𝜂. (16.50) (16.51) (16.52) (16.53) (16.54) (16.55) Here, only one linear term is left for shear strain components such that the modes causing shear locking are removed. The normal strain components keep all non- constant terms given in equation (16.48). Summation of equation (16.49) and equations (16.50)–(16.55) yields the following strain submatrices which can eliminate the shear and volumetric locking: B̅̅̅̅̅𝑥𝑥(𝜉 , 𝜂, 𝜁 ) = B̅̅̅̅̅𝑥𝑥(0) + B̅̅̅̅̅𝑥𝑥,𝜉 +B̅̅̅̅̅𝑥𝑥,𝜉𝜂 dev (0)𝜉𝜂 + B̅̅̅̅̅𝑥𝑥,𝜂𝜁 dev (0)𝜉 + B̅̅̅̅̅𝑥𝑥,𝜂 dev (0)𝜁𝜉 , dev (0)𝜂𝜁 + B̅̅̅̅̅𝑥𝑥,𝜁𝜉 dev (0)𝜂 + B̅̅̅̅̅𝑥𝑥,𝜁 dev (0)𝜁 B̅̅̅̅̅𝑦𝑦(𝜉 , 𝜂, 𝜁 ) = B̅̅̅̅̅𝑦𝑦(0) + B̅̅̅̅̅𝑦𝑦,𝜉 +B̅̅̅̅̅𝑦𝑦,𝜉𝜂 dev (0)𝜉𝜂 + B̅̅̅̅̅𝑦𝑦,𝜂𝜁 dev (0)𝜉 + B̅̅̅̅̅𝑦𝑦,𝜂 dev (0)𝜁𝜉 , dev (0)𝜂𝜁 + B̅̅̅̅̅𝑦𝑦,𝜁𝜉 dev (0)𝜂 + B̅̅̅̅̅𝑦𝑦,𝜁 dev (0)𝜁 (16.56) (16.57) LS-DYNA Theory Manual Eight-Node Solid Element for Thick Shell Simulations B̅̅̅̅̅𝑧𝑧(𝜉 , 𝜂, 𝜁 ) = B̅̅̅̅̅𝑧𝑧(0) + B̅̅̅̅̅𝑧𝑧,𝜉 +B̅̅̅̅̅𝑧𝑧,𝜉𝜂 dev (0)𝜉𝜂 + B̅̅̅̅̅𝑧𝑧,𝜂𝜁 dev (0)𝜂𝜁 + B̅̅̅̅̅𝑧𝑧,𝜁𝜉 dev (0)𝜁𝜉 , dev(0)𝜉 + B̅̅̅̅̅𝑧𝑧,𝜂 dev(0)𝜂 + B̅̅̅̅̅𝑧𝑧,𝜁 dev(0)𝜁 B̅̅̅̅̅𝑥𝑦(𝜉 , 𝜂, 𝜁 ) = B̅̅̅̅̅𝑥𝑦(0) + B̅̅̅̅̅𝑥𝑦,𝜁 dev (0)𝜁 , B̅̅̅̅̅𝑦𝑧(𝜉 , 𝜂, 𝜁 ) = B̅̅̅̅̅𝑦𝑧(0) + B̅̅̅̅̅𝑦𝑧,𝜉 dev (0)𝜉 , B̅̅̅̅̅𝑧𝑥(𝜉 , 𝜂, 𝜁 ) = B̅̅̅̅̅𝑧𝑥(0) + B̅̅̅̅̅𝑧𝑥,𝜂 dev (0)𝜂. (16.58) (16.59) (16.60) (16.61) It is noted that the elements developed above cannot pass the patch test if the elements are skewed. To remedy this drawback, the gradient vectors defined in (16.18)– (16.20) are replaced by the uniform gradient matrices, proposed by Flanagan [1981], b̃ ⎡ b̃ ⎢⎢ b̃ ⎣ ⎤ ⎥⎥ 3⎦ = 𝑉𝑒 ∫ Ω𝑒 B1(𝜉 , 𝜂, 𝜁 ) ⎤ ⎡ B2(𝜉 , 𝜂, 𝜁 ) ⎥ ⎢ B3(𝜉 , 𝜂, 𝜁 )⎦ ⎣ 𝑑𝑉 . Where 𝑉𝑒 is the element volume and the stabilization vector are redefined as 𝛄̃𝛼 = 𝐡𝛼 − (𝐡𝛼 T𝐱𝑖)𝐛̃ 𝑖. (16.62) (16.63) The element using the strain submatrices (16.56)-(16.61) and uniform gradient matrices (16.62) with four-point quadrature scheme is called HEXDS element. g2 e^ g1 e^ e^ ζ = 0 Figure 16.1. Definition of co-rotational coordinate system Eight-Node Solid Element for Thick Shell Simulations LS-DYNA Theory Manual 16.3.2 Co-rotational Coordinate System In elements for shell/plate structure simulations, the elimination of the shear locking depends on the proper treatment of the shear strain. It is necessary to attach a local coordinate system to the element so that the strain tensor in this local system is relevant for the treatment. The co-rotational coordinate system determined here is one of the most convenient ways to define such a local system. A co-rotational coordinate system is defined as a Cartesian coordinate system which rotates with the element. Let {𝑥𝑎, 𝑦𝑎, 𝑧𝑎} denote the current nodal spatial coordinates in the global system. For each quadrature point with natural coordi- nates(𝜉 , 𝜂, 𝜁 ), we can have two tangent directions on the mid-surface (𝜁 = 0) within the element 𝐠1 = 𝐠2 = ∂𝐱 ∂𝜉 ∂𝐱 ∂𝜂 = [ ∂𝑥 ∂𝜉 ∂𝑦 ∂𝜉 ∂𝑧 ∂𝜉 = [ ∂𝑥 ∂𝜂 ∂𝑦 ∂𝜂 ∂𝑧 ∂𝜂 ] = [𝑁𝑎,𝜉 𝑥𝑎 𝑁𝑎,𝜉 𝑦𝑎 𝑁𝑎,𝜉 𝑧𝑎](𝜉,𝜂,0), ] = [𝑁𝑎,𝜂𝑥𝑎 𝑁𝑎,𝜂𝑦𝑎 𝑁𝑎,𝜂𝑧𝑎](𝜉,𝜂,0). (16.64) (16.65) The unit vector 𝐞̂1 of the co-rotational coordinate system is defined as the bisector of the angle intersected by these two tangent vectors 𝐠1 and 𝐠2; the unit vector 𝐞̂3 is perpendicular to the mid-surface and the other unit vector is determined by 𝐞̂1 and 𝐞̂3, i.e., 𝐞̂1 = ( 𝐠1 ∣𝐠1∣ + 𝐠2 ∣𝐠2∣ ⁄ ) (∣ 𝐠1 ∣𝐠1∣ + 𝐠2 ∣𝐠2∣ , ∣) 𝐞̂3 = 𝐠1 × 𝐠2 ∣𝐠1 × 𝐠2∣ , 𝐞̂2 = 𝐞̂3 × 𝐞̂1, which lead to the transformation matrix 𝐑 = 𝐞̂1 ⎤. ⎡ 𝐞̂2 ⎥ ⎢ 𝐞̂3⎦ ⎣ (16.66) (16.67) (16.68) (16.69) 16.3.3 Stress and Strain Measures Since the co-rotational coordinate system rotates with the configuration, the stress defined in this co-rotational system does not change with the rotation or translation of the material body and is thus objective. Therefore, we use the Cauchy stress in the co-rotational coordinate system, called the co-rotational Cauchy stress, as our stress measure. LS-DYNA Theory Manual Eight-Node Solid Element for Thick Shell Simulations The rate of deformation (or velocity strain tensor), also defined in the co- rotational coordinate system, is used as the measure of the strain rate, 𝛆̇ = 𝐝̂ = ⎡∂𝐯̂def ⎢ ∂𝐱̂ ⎣ + ( ∂𝐯̂def ∂𝐱̂ ) ⎤, ⎥ ⎦ (16.70) where 𝐯̂def is the deformation part of the velocity in the co-rotational system 𝐱̂. If the initial strain 𝛆̂ (𝐗, 0) is given, the strain tensor can be expressed as, 𝛆̂(X, 𝑡) = 𝛆̂(𝐗, 0) + ∫ 𝐝̂(𝐗, 𝜏) 𝑑𝜏. (16.71) The strain increment is then given by the mid-point integration of the velocity strain tensor, 𝑡𝑛+1 𝐝̂𝑑𝜏 =̇ Δ𝛆̂ = ∫ 𝑡𝑛 ⎡∂Δ𝐮̂def ⎢⎢ ∂𝐱̂ ⎣ + ⎜⎜⎜⎛∂Δ𝐮̂def ⎟⎟⎟⎞ 2 ⎠ ∂𝐱̂ ⎤ , ⎥⎥ ⎦ 𝑛+1 where Δ𝐮̂def is the deformation part of the displacement increment in the co-rotational system 𝐱̂𝑛 + 1 referred to the mid-point configuration. 𝑛+1 ⎝ (16.72) 16.3.4 Co-rotational Stress and Strain Updates For stress and strain updates, we assume that all variables at the previous time step 𝑡𝑛 are known. Since the stress and strain measures defined in the earlier section are objective in the co-rotational system, we only need to calculate the strain increment from the displacement field within the time increment [𝑡𝑛, 𝑡𝑛 + 1]. The stress is then updated by using the radial return algorithm. All the kinematical quantities must be computed from the last time step configuration, Ω𝑛, at 𝑡 = 𝑡𝑛 and the current configuration, Ω𝑛 + 1 at 𝑡 = 𝑡𝑛 + 1 since these are the only available data. Denoting the spatial coordinates of these two configurations as 𝐱nand 𝐱n + 1 in the fixed global Cartesian coordinate system 𝑂x, as shown in Figure 16.2, the coordinates in the corresponding co-rotational Cartesian coordinate systems, 𝑂𝐱̂𝑛 and 𝑂𝐱̂𝑛 + 1, can be obtained by the following transformation rules: 𝐱̂𝑛 = 𝐑𝑛𝐱𝑛, 𝐱̂𝑛+1 = 𝐑𝑛+1𝐱𝑛+1, (16.73) (16.74) where 𝐑𝑛 and 𝐑𝑛 + 1 are the orthogonal transformation matrices which rotate the global coordinate system to the corresponding co-rotational coordinate systems, respectively. Eight-Node Solid Element for Thick Shell Simulations LS-DYNA Theory Manual n+1 n+1/2 ^ n+1 ^ n+1/2 ^ Xn Figure 16.2. Configurations at times 𝑡𝑛, 𝑡𝑛 + 1 , and 𝑡𝑛+1, Since the strain increment is referred to the configuration at 𝑡 = 𝑡𝑛 + 1 assuming the velocities within the time increment [𝑡𝑛, 𝑡𝑛 + 1] are constant, we have , by = 𝑛+1 (𝐱𝑛 + 𝐱𝑛+1), (16.75) and the transformation to the co-rotational system associated with this mid-point configuration, Ω𝑛 + 1 , is given by 𝐱̂ 𝑛+1 = 𝐑 𝑛+1 . 𝑛+1 (16.76) Similar to polar decomposition, an incremental deformation can be separated into the summation of a pure deformation and a pure rotation [Belytschko, 1973]. Letting Δ𝐮 indicate the displacement increment within the time increment [𝑡𝑛, 𝑡𝑛 + 1 we write ], Δ𝐮 = Δ𝐮def + Δ𝐮rot, (16.77) where Δ𝐮def and Δ𝐮rot are, respectively, the deformation part and the pure rotation part of the displacement increment in the global coordinate system. The deformation part also includes the translation displacements which cause no strains. LS-DYNA Theory Manual Eight-Node Solid Element for Thick Shell Simulations In order to obtain the deformation part of the displacement increment referred to , we need to find the rigid rotation from Ω𝑛 to Ω𝑛 + 1 , is held still. Defining two virtual the configuration at 𝑡 = 𝑡𝑛 + 1 provided that the mid-point configuration, Ω𝑛 + 1 configurations, Ω′𝑛 and Ω′𝑛 + 1, by rotating the element bodies Ω𝑛 and Ω𝑛 + 1 into the (Fig. 13.3) and denoting and 𝐱′̂ co-rotational system 𝑂x̂𝑛 + 1 𝑛 + 1 as the coordinates of Ω′𝑛 and Ω′𝑛 + 1 in the co-rotational system 𝑂𝐱̂𝑛 + 1 , we have 𝐱′̂ 𝑛 = 𝐱̂𝑛, 𝐱′̂ 𝑛 + 1 = 𝐱̂𝑛 + 1. (16.78) We can see that from Ω𝑛 to Ω′𝑛 and from Ω′𝑛 + 1 to Ω𝑛 + 1, the body experiences two rigid rotations and the rotation displacements are given by Δ𝐮1 rot = 𝐱′𝑛 − 𝐱𝑛 = 𝐑 𝑛 − 𝐱𝑛 = 𝐑 T 𝐱′̂ 𝑛+1 T 𝐱̂𝑛 − 𝐱𝑛, 𝑛+1 Δ𝐮2 rot = 𝐱𝑛+1 − 𝐱′𝑛+1 = 𝐱𝑛+1 − 𝐑 𝑛+1 = 𝐱𝑛+1 − 𝐑 T 𝐱′̂ 𝑛+1 T 𝐱̂𝑛+1. 𝑛+1 Thus the total rotation displacement increment can be expressed as T (𝐱̂𝑛+1 − 𝐱̂𝑛) 𝑛+1 rot = 𝐱𝑛+1 − 𝐱𝑛 − 𝐑 Δ𝐮rot = Δ𝐮1 rot + Δ𝐮2 = Δ𝐮 − 𝐑 T (𝐱̂𝑛+1 − 𝐱̂𝑛). 𝑛+1 (16.79) (16.80) (16.81) Then the deformation part of the displacement increment referred to the configuration Ω𝑛 + 1 is Δ𝐮def = Δ𝐮 − Δ𝐮rot = 𝐑 T (𝐱̂𝑛+1 − 𝐱̂𝑛). 𝑛+1 (16.82) Therefore, the deformation displacement increment in the co-rotational coordinate system 𝑂x̂𝑛 + 1 is obtained as Δ𝐮̂def = 𝐑 𝑛+1 Δ𝐮def = 𝐱̂𝑛+1 − 𝐱̂𝑛. (16.83) Once the strain increment is obtained by equation (16.72), the stress increment, also referred to the mid-point Configuration, can be calculated with the radial return algorithm. The total strain and stress can then be updated as 𝛆̂𝑛+1 = 𝛆̂𝑛 + Δ𝛆̂, 𝛔̂𝑛+1 = 𝛔̂𝑛 + Δ𝛔̂. (16.84) (16.85) Eight-Node Solid Element for Thick Shell Simulations LS-DYNA Theory Manual n+1 Δu Pn+1 rot Δu2 , n+1 n+1/2 Δudef n+1 ^ Ω, n+1 ^ n+1/2 , Ω, rot Δu1 Pn ^ Figure 16.3. Separation of the displacement increment Note that the resultant stress and strain tensors are both referred to the current configuration and defined in the current co-rotational coordinate system. By using the tensor transformation rule we can have the strain and stress components in the global coordinate system. Tangent Stiffness Matrix and Nodal Force Vectors From the Hu-Washizu variational principle, at both 𝑣th and (𝑣 + 1)th iteration, we have ∫ 𝛿𝜀̂𝑖𝑗 Ω̂𝑣 𝑣 𝜎̂𝑖𝑗 𝑣 , 𝑑𝑉 = 𝛿𝜋̂ext ∫ Ω̂𝑣+1 𝛿𝜀̂𝑖𝑗 𝑣+1𝜎̂𝑖𝑗 𝑣+1 𝑑𝑉 = 𝛿𝜋̂ext 𝑣+1, (16.86) (16.87) where 𝛿𝜋̂ext is the virtual work done by the external forces. Note that both equations are written in the co-rotational coordinate system defined in the 𝑣th iterative configuration given by x𝑛+1 . The variables in this section are within the time step [𝑡𝑛, 𝑡𝑛+1 ] and superscripts indicate the number of iterations. Assuming that all external forces are deformation-independent, linearization of Equation (16.87) gives [Liu, 1992] LS-DYNA Theory Manual Eight-Node Solid Element for Thick Shell Simulations ∫ 𝛿𝑢̂𝑖,𝑗 Ω̂𝑣 𝑣 𝐶̂ 𝑣 Δ𝑢̂𝑘,𝑙𝑑𝑉 + 𝑖𝑗𝑘𝑙 ∫ 𝛿𝑢̂𝑖,𝑗 Ω̂𝑣 𝑣 𝑇̂ 𝑣 Δ𝑢̂𝑘,𝑙𝑑𝑉 = 𝛿𝜋̂ext 𝑖𝑗𝑘𝑙 𝑣+1 − 𝑣 , 𝛿𝜋̂ext where the Green-Naghdi rate of Cauchy stress tensor is used, i.e., 𝑇̂ 𝑣. 𝑣 = 𝛿𝑖𝑘𝜎̂𝑗𝑙 𝑖𝑗𝑘𝑙 (16.88) (16.89) The first term on the left hand side of (16.88) denotes the material response since it is due to pure deformation or stretching; the second term is an initial stress part resulting from finite deformation effect. Taking account of the residual of the previous iteration, Equation (16.87) can be approximated as ∫ 𝛿𝑢̂𝑖,𝑗 Ω̂𝑣 𝑣 (𝐶̂ 𝑣 + 𝑇̂ 𝑖𝑗𝑘𝑙 𝑣 )Δ𝑢̂𝑘,𝑙 𝑖𝑗𝑘𝑙 𝑑𝑉 = 𝛿𝜋̂ext 𝑣+1 − ∫ 𝛿𝜀̂𝑖𝑗 𝑣 𝜎̂𝑖𝑗 𝑣𝑑𝑉 Ω̂𝑣 . (16.90) If the strain and stress vectors are defined as 𝛆T = [𝜀𝑥 𝜀𝑦 𝜀𝑧 2𝜀𝑥𝑦 2𝜀𝑦𝑧 2𝜀𝑧𝑥 2𝜔𝑥𝑦 2𝜔𝑦𝑧 2𝜔𝑧𝑥], 𝛔T = [𝜎𝑥 𝜎𝑦 𝜎𝑧 𝜎𝑥𝑦 𝜎𝑦𝑧 𝜎𝑧𝑥], (16.91) (16.92) We can rewrite equation (16.90) as ∫ 𝛿𝜀̂𝑖 Ω̂𝑣 𝑣(𝐶̂𝑖𝑗 𝑣 + 𝑇̂𝑖𝑗 𝑣)𝛿𝜀̂𝑗 𝑑𝑉 = 𝛿𝜋̂ext 𝑣+1 − ∫ 𝛿𝜀̂𝑖 𝑣𝜎̂𝑗 𝑣𝑑𝑉 Ω̂𝑣 , (16.93) 𝑣 is the consistent tangent modulus tensor corresponding to pure deformation 𝑣 is the geometric stiffness matrix where 𝐶̂𝑖𝑗 but expanded to a 9 by 9 matrix; 𝑇̂𝑖𝑗 which is given as follows [Liu 1992]: Eight-Node Solid Element for Thick Shell Simulations LS-DYNA Theory Manual 𝜎2 𝜎3 𝜎4 𝜎4 𝜎1 + 𝜎2 𝜎5 𝜎5 𝜎6 𝜎2 + 𝜎3 symm. 𝜎6 𝜎6 𝜎5 𝜎4 𝜎1 + 𝜎3 𝜎4 𝜎4 − 𝜎2 − 𝜎1 𝜎6 − 𝜎5 𝜎1 + 𝜎2 T = ⎡𝜎1 ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎣ 𝜎5 𝜎5 − 𝜎6 𝜎3 − 𝜎2 𝜎4 𝜎6 𝜎2 + 𝜎3 − − − 𝜎6 𝜎6 𝜎5 − 𝜎4 𝜎1 − 𝜎3 𝜎5 𝜎4 𝜎3 + 𝜎1 − − (16.94) ⎤ ⎥ ⎥ ⎥ ⎥ ⎥ ⎥ ⎥ ⎥ ⎥ ⎥ ⎥ . ⎥ ⎥ ⎥ ⎥ ⎥ ⎥ ⎥ ⎥ ⎥ ⎥ ⎥ ⎦ By interpolation Δ𝐮 = 𝐍Δ𝐝, 𝛿𝐮 = 𝐍𝛿𝐝; (16.95) (16.96) where 𝐍 and 𝐁̅̅̅̅̅ are, respectively, the shape functions and strain operators defined in Section 2. This leads to a set of equations Δ𝛆 = 𝐁̅̅̅̅̅Δ𝐝, 𝛿𝛆 = 𝐁̅̅̅̅̅𝛿𝐝, 𝐊̂𝑣Δ𝐝̂ = 𝐫 ̂𝑣+1 = 𝐟 ̂ 𝑣+1 − 𝐟 ̂ ext 𝑣 , int (16.97) where the tangent stiffness matrix, 𝐊̂𝑣, and the internal nodal force vector, 𝐟 ̂ 𝑣 , are int 𝐊̂𝑣 = ∫ 𝐁̅̅̅̅̅̂T(𝐂̂𝑣 + 𝐓̂𝑣)𝐁̅̅̅̅̅̂dV Ω̂𝑣 , 𝑣 = ∫ 𝐁̅̅̅̅̅̂T𝛔̂𝑣dV 𝐟 ̂ int Ω̂𝑣 . (16.98) (16.99) The tangent stiffness and nodal force are transformed into the global coordinate system tensorially as 𝐊𝑣 = 𝐑𝑣T𝐊̂𝑣𝐑𝑣, 𝑣 , 𝐫𝑣+1 = 𝐑𝑣T𝐫 ̂int (16.100) (16.101) where 𝐑𝑣 is the transformation matrix of the co-rotational system defined by 𝐱𝑛+1 Finally, we get a set of linear algebraic equations . LS-DYNA Theory Manual Eight-Node Solid Element for Thick Shell Simulations 𝐊𝑣Δ𝐝𝑣+1 = 𝐫𝑣+1. (16.102) 16.4 Numerical Examples To investigate the performance of the element introduced in this paper, a variety of problems including linear elastic and nonlinear elastic-plastic/large deformation problems are studied. Since the element is developed to avoid locking, the applicability to problems of thin structures is studied by solving the standard test problems including pinched cylinder and Scordelis-Lo roof, which are proposed by MacNeal, 1985 and Belytschko, 1984b. Also a sheet metal forming problem is solved to test and demonstrate the effectiveness and efficiency of this element. 16.4.1 Timoshenko Cantilever Beam The first problem is a linear, elastic cantilever beam with a load at its end as shown in Fig. 16.4, where 𝑀 and 𝑃 at the left end of the cantilever are reactions at the support. The analytical solution from Timoshenko, 1970 is 𝑢𝑥(𝑥, 𝑦) = −𝑃𝑦 6𝐸̅̅̅̅𝐼 [(6𝐿 − 3𝑥)𝑥 + (2 + 𝑣̅) (𝑦2 − 𝐷2)], (16.103) 𝑢𝑦(𝑥, 𝑦) = 6𝐸̅̅̅̅𝐼 [3𝑣̅𝑦2(𝐿 − 𝑥) + (4 + 5𝑣̅)𝐷2𝑥 + (3𝐿 − 𝑥)𝑥2], (16.104) where 𝐼 = 12 𝐷3, 𝐸̅̅̅̅ = { 𝐸, 𝐸/(1 − 𝑣2) , 𝑣̅ = {⎧ ⎩{⎨ 1 − 𝑣 for plane stress for plane strain (16.105) (16.106) The displacements at the support end, 𝑥 = 0, − 1 2 𝐷 are nonzero except at the top, bottom and midline (as shown in Fig. 13.5). Reaction forces are applied at the support based on the stresses corresponding to the displacement field at 𝑥 = 0, which are 2 𝐷 ≤ 𝑦 ≤ 1 𝜎𝑥𝑥 = − 𝑃𝑦 (𝐿 − 𝑥), 𝜎𝑦𝑦 = 0, 𝜎𝑥𝑦 = 2𝐼 ( 𝐷2 − 𝑦2). (16.107) The distribution of the applied load to the nodes at 𝑥 = 𝐿 is also obtained from the closed-form stress fields. Eight-Node Solid Element for Thick Shell Simulations LS-DYNA Theory Manual Figure 16.4. Timoshenko cantilever beam. D/2 D/2 (a) Regular mesh L/4 (b) Skewed mesh p/2 Pt. A p/2 Pt. A Figure 16.5. Top half of anti-symmetric beam mesh The parameters for the cantilever beam are: 𝐿 = 1.0, 𝐷 = 0.02, 𝑃 = 2.0, 𝐸 = 1 × 107; and two values of Poisson’s ratio: (1)𝑣 = 0.25, (2)𝑣 = 0.4999. Since the problem is anti-symmetric, only the top half of the beam is modeled. Plane strain conditions are assumed in the z-direction and only one layer of elements is used in this direction. Both regular mesh and skewed mesh are tested for this problem. Normalized vertical displacements at point A for each case are given in Table 13.1. Tables 13.1a and 13.1b show the normalized displacement at point A for the LS-DYNA Theory Manual Eight-Node Solid Element for Thick Shell Simulations regular mesh. There is no shear or volumetric locking for this element. For the skewed mesh, with the skewed angle increased, we need more elements to get more accurate solution (Table 13.1c). (a) 𝑣 = 0.25, regular mesh Analytical solution 𝑤A = 9.3777 × 10−2 Mesh 4 × 1 × 1 8 × 1 × 1 8 × 2 × 1 HEXDS 1.132 1.142 1.029 (b) 𝑣 = 0.4999, regular mesh Analytical solution 𝑤A = 7.5044 × 10−2 Mesh 4 × 1 × 1 8 × 1 × 1 8 × 2 × 1 HEXDS 1.182 1.197 1.039 (c) 𝑣 = 0.25, skewed mesh 1° 5° 10° 4 × 1 ×1 8 × 1 ×1 1.078 0.580 0.317 1.136 0.996 0.737 16 × 1 ×1 1.142 1.090 .955 Table 13.1. Normalized displacement at point A of cantilever beam. Eight-Node Solid Element for Thick Shell Simulations LS-DYNA Theory Manual 16.4.2 Pinched Cylinder Figure 16.6 shows a pinched cylinder subjected to a pair of concentrated loads. Two cases are studied in this example. In the first case, both ends of the cylinder are assumed to be free. In the second case, both ends of the cylinder are covered with rigid diaphragms so that only the displacement in the axial direction is allowed at the ends. The parameters for the first case (without diaphragms) are 𝐸 = 1.05 × 106, 𝑣 = 0.3125, 𝐿 = 10.35, 𝑅 = 1.0, 𝑡 = 0.094, 𝑃 = 100.0; (16.108) while for the second case (with diaphragms), the parameters are set to be 𝐸 = 3 × 106, 𝑣 = 0.3, 𝐿 = 600.0, 𝑅 = 300.0, 𝑡 = 3.0, 𝑃 = 1.0. (16.109) Due to symmetry only one octant of the cylinder is modeled. The computed displacements at the loading point are compared to the analytic solutions in Table 13.2. HEXDS element works well in both cases, indicating that this element can avoid not only shear locking but also membrane locking; this is not unexpected since membrane locking occurs primarily in curved elements [Stolarski, 1983]. 16.4.3 Scordelis-Lo Roof Scordelis-Lo roof subjected to its own weight is shown in Figure 16.7. Both ends of the roof are assumed to be covered with rigid diaphragms. The parameters are selected to be: 𝐸 = 4.32 × 108, 𝑣 = 0.0, 𝐿 = 50.0, 𝑅 = 25.0, 𝑡 = 0.25, 𝜃 = 40∘, and the gravity is 360.0 per volume. free or with diaphragm m etric sy m symmetric m etric sy m Figure 16.6. Pinched cylinder and the element model LS-DYNA Theory Manual Eight-Node Solid Element for Thick Shell Simulations 2L Figure 16.7. Scordelis-Lo roof under self-weight (a) First case without diaphragms Analytical solution 𝑤max = 0.1137 Mesh 10 × 10 × 2 16 × 16 × 4 20 × 20 × 4 HEXDS 1.106 1.054 1.067 (b) Second case with diaphragms Analytical solution wmax = 1.8248 × 10−5 Mesh 10 × 10 × 2 16 × 16 × 4 20 × 20 × 4 HEXDS 0.801 0.945 .978 Table 13.2. Normalized displacement at loading point of pinched cylinder Due to symmetry only one quarter of the roof is modeled. The computed displacement at the midpoint of the edge is compared to the analytic solution in Table 13.3. In this example the HEXDS element can get good result with 100 × 2 elements. Eight-Node Solid Element for Thick Shell Simulations LS-DYNA Theory Manual R0=50.8mm t=2mm tight die r=2mm Rd=54mm R=54mm Figure 16.8. Circular sheet stretched with a tight die Analytical solution 𝑤max = 0.3024 Mesh 8 × 8 × 1 16 × 16 × 1 32 × 32 × 1 10 × 10 × 2 HEXDS 1.157 1.137 1.132 1.045 16.4.4 Circular Sheet Stretched with a Tight Die A circular sheet is stretched under a hemisphere punch and a tight die with a small corner radius (Fig. 16.8). The material is elastoplastic with nonlinear hardening rule. The elastic material constants are: 𝐸 = 206 GPa and 𝑣 = 0.3. In the plastic range, the uniaxial stress-strain curve is given by 𝜎 = 𝐾𝜀𝑛, (16.110) where 𝐾 = 509.8MPa, 𝑛 = 0.21, 𝜎 is Cauchy stress and 𝜀 is natural strain (logarithmic strain). The initial yield stress is obtained to be 𝜎0 = 103.405Mpa and the tangent modulus at the initial yield point is 𝐸t = 0.4326 × 105MPa. Because of the small corner radius of the die, the same difficulties as in the problem of sheet stretch under the rigid cylinders lead the shell elements to failure in this problem. Three-dimensional solid elements are needed and fine meshes should be put in the areas near the center and the edge of the sheet. One quarter of the sheet is modeled with 1400 × 2 HEXDS elements due to the double symmetries. The mesh is shown in Fig. 16.9. Two layers of elements are used in the thickness. Around the center and near the circular edge of the sheet, fine mesh is used. The nodes on the edge are fixed in x- and y-directions and the bottom nodes on the edge are prescribed in three directions. No friction is considered in this simulation. LS-DYNA Theory Manual Eight-Node Solid Element for Thick Shell Simulations Figure 16.9. Mesh for circular sheet stretching For comparison, the axisymmetric four-node element with reduced integration (CAX4R) is also used and the mesh for this element is the same as shown in the top of Figure 13.9. The results presented here are after the punch has traveled down 50 mm. The profile of the circular sheet is shown in Figure 16.10 where we can see that the sheet Figure 16.10. Deformed shape of a circular sheet with punch travel 50 mm under the punch experiences most of the stretching and the thickness of the sheet above Eight-Node Solid Element for Thick Shell Simulations LS-DYNA Theory Manual Figure 16.11. Reaction force vs. punch travel for the circular sheet the die changes a lot. The deformation between the punch and the die is small. However, the sheet thickness obtained by the CAX4R element is less than that by the HEXDS element and there is slight difference above the die. These observations can be verified by the strain distributions in the sheet along the radial direction (Figure 13.12). The direction of the radial strain is the tangent of the mid-surface of the element in the rz plane and the thickness strain is in the direction perpendicular to the mid-surface of the element. The unit vector of the circumferential strain is defined as the cross-product of the directional cosine vectors of the radial strain and the thickness strain. We can see that the CAX4R element yields larger strain components in the area under the punch than the HEXDS element. The main difference of the strain distributions in the region above the die is that the CAX4R element gives zero circumferential strain in this area but the HEXDS element yields non-zero strain. The value of the reaction force shown in the Figure 13.11 is only one quarter of the total punch reaction force since only one quarter of the sheet is modeled. From this figure we can see that the sheet begins softening after the punch travels down about 45 mm, indicating that the sheet may have necking though this cannot be seen clearly from Figure 16.10. LS-DYNA Theory Manual Eight-Node Solid Element for Thick Shell Simulations (a) Radial strain distribution (b) Circumferential strain distribution (c) Thickness strain distribution Figure 13.12. Strain distributions in circular sheet with punch travel 50 mm Eight-Node Solid Element for Thick Shell Simulations LS-DYNA Theory Manual 16.5 Conclusions A new eight-node hexahedral element is implemented for the large deformation elastic-plastic analysis. Formulated in the co-rotational coordinate system, this element is shown to be effective and efficient and can achieve fast convergence in solving a wide variety of nonlinear problems. By using a co-rotational system which rotates with the element, the locking phenomena can be suppressed by omitting certain terms in the generalized strain operators. In addition, the integration of the constitutive equation in the co-rotational system takes the same simple form as small deformation theory since the stress and strain tensors defined in this co-rotational system are objective. Radial return algorithm is used to integrate the rate-independent elastoplastic constitutive equation. The tangent stiffness matrix consistently derived from this integration scheme is crucial to preserve the second order convergence rate of the Newton’s iteration method for the nonlinear static analyses. Test problems studied in this paper demonstrate that the element is suitable to continuum and structural numerical simulations. In metal sheet forming analysis, this element has advantages over shell elements for certain problems where through the thickness deformation and strains are significant. LS-DYNA Theory Manual Truss Element 17 Truss Element One of the simplest elements is the pin-jointed truss element shown in Figure 17.1. This element has three degrees of freedom at each node and carries an axial force. The displacements and velocities measured in the local system are interpolated along the axis according to 𝑢 = 𝑢1 + (𝑢2 − 𝑢1), where at 𝑥 = 0, 𝑢 = 𝑢1 and at 𝑥 = 𝐿, 𝑢 = 𝑢2. Incremental strains are found from (𝑢̇2 − 𝑢̇1), 𝑢̇ = 𝑢̇1 + and are computed in LS-DYNA using Δ𝜀 = (𝑢̇2 − 𝑢̇1) Δ𝑡 Δ𝜀𝑛+1 2⁄ = 2 (𝑢̇2 𝑛+1 2⁄ 𝑛+1 2⁄ − 𝑢̇1 𝐿𝑛 + 𝐿𝑛+1 ) Δ𝑡𝑛+1 2⁄ (17.1) (17.2) (17.3) (17.4) The normal force 𝑁 is then incrementally updated using a tangent modulus 𝐸𝑡 according to 𝑁𝑛+1 = N𝑛𝐴𝐸𝑡 + Δ𝜀𝑛+1/2 (17.5) Truss Element N1 LS-DYNA Theory Manual u1 N2 u2 Figure 17.1. Truss element. Two constitutive models are implemented for the truss element: elastic and elastic-plastic with kinematic hardening. LS-DYNA Theory Manual Membrane Element 18 Membrane Element The Belytschko-Lin-Tsay shell element {Belytschko and Tsay [1981], Belytschko et al., [1984a]} is the basis for this very efficient membrane element. In this section we briefly outline the theory employed which, like the shell on which it is based, uses a combined co-rotational and velocity-strain formulation. The efficiency of the element is obtained from the mathematical simplifications that result from these two kinematical assumptions. The co-rotational portion of the formulation avoids the complexities of nonlinear mechanics by embedding a coordinate system in the element. The choice of velocity strain or rate of deformation in the formulation facilitates the constitutive evaluation, since the conjugate stress is the more familiar Cauchy stress. In membrane elements the rotational degrees of freedom at the nodal points may be constrained, so that only the translational degrees-of-freedom contribute to the straining of the membrane. A triangular membrane element may be obtained by collapsing adjacent nodes of the quadrilateral. 18.1 Co-rotational Coordinates The mid-surface of the quadrilateral membrane element is defined by the location of the element’s four corner nodes. An embedded element coordinate system (Figure 7.1) that deforms with the element is defined in terms of these nodal coordinates. The co-rotational coordinate system follows the development in Section 7, Equations (7.1)—(7.3). Membrane Element LS-DYNA Theory Manual 18.2 Velocity-Strain Displacement Relations The co-rotational components of the velocity strain (rate of deformation) are given by: 𝑑 ̂ 𝑖𝑗 = ( ∂𝜐̂𝑖 ∂𝑥̂𝑗 + ∂𝜐̂𝑗 ∂𝑥̂𝑖 ), (18.1) The above velocity-strain relations are evaluated only at the center of the shell. Standard bilinear nodal interpolation is used to define the mid-surface velocity, angular These velocity, and the element’s coordinates (isoparametric representation). interpolation relations are given by 𝑣𝑚 = 𝑁𝐼(𝜉 , 𝜂)𝑣𝐼, 𝑥𝑚 = 𝑁𝐼(𝜉 , 𝜂)𝑥𝐼, (18.2) (18.3) where the subscript 𝐼 is summed over all the element’s nodes and the nodal velocities are obtained by differentiating the nodal coordinates with respect to time, i.e., 𝜐𝐼 = ẋ𝐼. The bilinear shape functions are defined in Equations (7.10). The velocity strains at the center of the element, i.e., at 𝜉 = 0, and 𝜂 = 0, are obtained as in Section 7 giving: where 𝑑 ̂ 𝑥 = 𝐵1𝐼𝜐̂𝑥𝐼, 𝑑 ̂ 𝑦 = 𝐵2𝐼𝜐̂𝑦𝐼, 2𝑑 ̂ 𝑥𝑦 = 𝐵2𝐼𝑣̂𝑥𝐼 + 𝐵1𝐼𝑣̂𝑦𝐼, 𝐵1𝐼 = 𝐵2𝐼 = ∂𝑁𝐼 ∂𝑥̂ , ∂𝑁𝐼 ∂𝑦̂ . (18.4) (18.5) (18.6) (18.7) (18.8) 18.3 Stress Resultants and Nodal Forces After suitable constitutive evaluations using the above velocity strains, the resulting stresses are multiplied by the thickness of the membrane, h, to obtain local resultant forces. Therefore, 18-2 (Membrane Element) 𝑓 ̂ 𝑅 = ℎ𝜎̂𝛼𝛽, 𝛼𝛽 LS-DYNA Theory Manual Membrane Element where the superscript R indicates a resultant force and the Greek subscripts emphasize the limited range of the indices for plane stress plasticity. The above element centered force resultants are related to the local nodal forces by 𝑅 + 𝐵2𝐼𝑓 ̂ 𝑥𝐼 = 𝐴(𝐵1𝐼𝑓 ̂ 𝑓 ̂ 𝑅 ), 𝑥𝑦 𝑥𝑥 𝑅 + 𝐵1𝐼𝑓 ̂ 𝑦𝐼 = 𝐴(𝐵2𝐼𝑓 ̂ 𝑓 ̂ 𝑅 ), 𝑥𝑦 𝑦𝑦 (18.10) (18.11) where 𝐴 is the area of the element. The above local nodal forces are then transformed to the global coordinate system using the transformation relations given in Equation (7.5a). 18.4 Membrane Hourglass Control Hourglass deformations need to be resisted for the membrane element. The hourglass control for this element is discussed in Section 7.4. LS-DYNA Theory Manual Discrete Elements and Masses 19 Discrete Elements and Masses The discrete elements and masses in LS-DYNA provide a capability for modeling simple spring-mass systems as well as the response of more complicated mechanisms. Occasionally, the response of complicated mechanisms or materials needs to be included in LS-DYNA models, e.g., energy absorbers used in passenger vehicle bumpers. These mechanisms are often experimentally characterized in terms of force- displacement curves. LS-DYNA provides a selection of discrete elements that can be used individually or in combination to model complex force-displacement relations. The discrete elements are assumed to be massless. However, to solve the equations of motion at unconstrained discrete element nodes or nodes joining multiple discrete elements, nodal masses must be specified at these nodes. LS-DYNA provides a direct method for specifying these nodal masses in the model input. All of the discrete elements are two-node elements, i.e., three-dimensional springs or trusses. A discrete element may be attached to any of the other LS-DYNA continuum, structural, or rigid body element. The force update for the discrete elements may be written as 𝐟 ̂𝑖+1 = 𝐟 ̂𝑖 + Δ𝐟 ̂, (19.1) where the superscript 𝑖 + 1 indicates the time increment and the superposed caret (⋅ ̂) indicates the force in the local element coordinates, i.e., along the axis of the element. In the default case, i.e., no orientation vector is used; the global components of the discrete element force are obtained by using the element’s direction cosines: {⎧𝐹𝑥 }⎫ 𝐹𝑦 𝐹𝑧⎭}⎬ ⎩{⎨ = 𝑓 ̂ {⎧Δ𝑙𝑥 }⎫ Δ𝑙𝑦 }⎬ {⎨ Δ𝑙𝑧⎭ ⎩ {⎧𝑛𝑥 }⎫ = 𝑓 ̂ 𝑛𝑦 𝑛𝑧⎭}⎬ ⎩{⎨ = 𝑓 ̂𝐧 ~ , (19.2) where Discrete Elements and Masses LS-DYNA Theory Manual Δ𝐥 = {⎧Δ𝑙𝑥 }⎫ Δ𝑙𝑦 }⎬ {⎨ Δ𝑙𝑧⎭ ⎩ = {⎧𝑥2 − 𝑥1 }⎫ 𝑦2 − 𝑦1 𝑧2 − 𝑧1 ⎭}⎬ ⎩{⎨ . 𝑙 is the length 𝑙 = √Δ𝑙𝑥 2 + Δ𝑙𝑦 2, 2 + Δ𝑙𝑧 (19.3) (19.4) and (𝑥𝑖, 𝑦𝑖, 𝑧𝑖) are the global coordinates of the nodes of the spring element. The forces in Equation (19.2) are added to the first node and subtracted from the second node. For a node tied to ground we use the same approach but for the (𝑥2, 𝑦2, 𝑧2) coordinates in Equation (19.2) the initial coordinates of node 1, i.e., (𝑥0, 𝑦0, 𝑧0) are used instead; therefore, {⎧𝐹𝑥 }⎫ 𝐹𝑦 𝐹𝑧⎭}⎬ ⎩{⎨ = 𝑓 ̂ {⎧𝑥0 − 𝑥1 }⎫ 𝑦0 − 𝑦1 𝑧0 − 𝑧1 ⎭}⎬ ⎩{⎨ {⎧𝑛𝑥 }⎫ = 𝑓 ̂ 𝑛𝑦 𝑛𝑧⎭}⎬ ⎩{⎨ . (19.5) The increment in the element force is determined from the user specified force- force-displacement/velocity Currently, nine types of displacement relation. relationships may be specified: 1. 2. 3. 4. 5. 6. 7. 8. 9. linear elastic; linear viscous; nonlinear elastic; nonlinear viscous; elasto-plastic with isotropic hardening; general nonlinear; linear viscoelastic. inelastic tension and compression only. muscle model. The force-displacement relations for these models are discussed in the following later. 19.1 Orientation Vectors An orientation vector, {⎧𝑚1 }⎫ 𝑚2 𝑚3⎭}⎬ ⎩{⎨ can be defined to control the direction the spring acts. If orientation vectors are used, it is strongly recommended that the nodes of the discrete element be coincident and 𝐦 = (19.6) , LS-DYNA Theory Manual Discrete Elements and Masses remain approximately so throughout the calculation. If the spring or damper is of finite length, rotational constraints will appear in the model that can substantially affect the results. If finite length springs are needed with directional vectors, then the discrete beam elements, the type 6 beam, should be used with the coordinate system flagged for the finite length case. We will first consider the portion of the displacement that lies in the direction of the vector. The displacement of the spring is updated based on the change of length given by where 𝐼0 is the initial length in the direction of the vector and lis the current length given for a node to node spring by Δ𝐼 = 𝐼 − 𝐼0, (19.7) 𝐼 = 𝑚1(𝑥2 − 𝑥1) + 𝑚2(𝑦2 − 𝑦1) + 𝑚3(𝑧2 − 𝑧1), and for a node to ground spring by 𝐼 = 𝑚1(𝑥0 − 𝑥1) + 𝑚2(𝑦0 − 𝑦1) + 𝑚3(𝑧0 − 𝑧1), (19.8) (19.9) The latter case is not intuitively obvious and can affect the sign of the force in unexpected ways if the user is not familiar with the relevant equations. The nodal forces are then given by {⎧𝐹𝑥 }⎫ 𝐹𝑦 𝐹𝑧⎭}⎬ ⎩{⎨ {⎧𝑚1 }⎫ = 𝑓 ̂ 𝑚2 𝑚3⎭}⎬ ⎩{⎨ . (19.10) The orientation vector can be either permanently fixed in space as defined in the input or acting in a direction determined by two moving nodes which must not be coincident but may be independent of the nodes of the spring. In the latter case, we recompute the direction every cycle according to: 𝑛 − 𝑥1 {⎧𝑥2 }⎫ 𝑛 − 𝑦1 𝑦2 𝑛 ⎭}⎬ ⎩{⎨ 𝑛 − 𝑧1 𝑧2 {⎧𝑚1 }⎫ 𝑚2 𝑚3⎭}⎬ ⎩{⎨ In Equation (19.9) the superscript, 𝑛, refers to the orientation nodes. 𝑙𝑛 (19.11) = . For the case where we consider motion in the plane perpendicular to the orientation vector we consider only the displacements in the plane, Δ𝑙𝑝, given by, Δ𝐥𝑝 = Δ𝐥 − 𝐦(𝐦 ⋅ Δ𝐥). (19.12) We update the displacement of the spring based on the change of length in the plane given by (19.13) 𝑝 is the initial length in the direction of the vector and 𝑙 is the current length 𝑝, Δ𝑙𝑝 = 𝑙𝑝 − 𝑙0 where 𝑙0 given for a node to node spring by Discrete Elements and Masses LS-DYNA Theory Manual 𝑙𝑝 = 𝑚1 𝑝(𝑥2 − 𝑥1) + 𝑚2 𝑝(𝑦2 − 𝑦1) + 𝑚3 𝑝(𝑧2 − 𝑧1), and for a node to ground spring by 𝑙𝑝 = 𝑚1 𝑝(𝑥0 − 𝑥1) + 𝑚2 𝑝(𝑦0 − 𝑦1) + 𝑚3 𝑝(𝑧0 − 𝑧1), where ⎧𝑚1 {{ 𝑚2 ⎨ {{ 𝑚3 ⎩ ⎫ }} ⎬ }} ⎭ = 𝑝 2 √Δ𝑙𝑥 𝑝 2 + Δ𝑙𝑦 𝑝 2 + Δ𝑙𝑧 ⎧Δ𝑙𝑥 {{ Δ𝑙𝑦 ⎨ {{ Δ𝑙𝑧 ⎩ ⎫ }} ⎬ }} ⎭ . After computing the displacements, the nodal forces are then given by {⎧𝐹𝑥 }⎫ 𝐹𝑦 𝐹𝑧⎭}⎬ ⎩{⎨ ⎧𝑚1 {{ = 𝑓 ̂ 𝑚2 ⎨ {{ 𝑚3 ⎩ ⎫ }} ⎬ }} ⎭ . (19.14) (19.15) (19.16) (19.17) 19.2 Dynamic Magnification “Strain Rate” Effects To account for “strain rate” effects, we have a simple method of scaling the forces based on the relative velocities that applies to all springs. The forces computed from the spring elements are assumed to be the static values and are scaled by an amplification factor to obtain the dynamic value: 𝐹dynamic = (1. + 𝑘𝑑 𝑉0 ) 𝐹static, (19.18) where 𝑘𝑑 = is a user defined input value 𝑉 = absolute relative velocity 𝑉0 = dynamic test velocity For example, if it is known that a component shows a dynamic crush force at 15 m/s equal to 2.5 times the static crush force, use 𝑘𝑑 = 1.5 and 𝑉0 = 15. 19.3 Deflection Limits in Tension and Compression The deflection limit in compression and tension is restricted in its application to no more than one spring per node subject to this limit, and to deformable bodies only. For example in the former case, if three spring are in series either the center spring or the two end springs may be subject to a limit but not all three. When the limiting LS-DYNA Theory Manual Discrete Elements and Masses deflection is reached momentum conservation calculations are performed and a common acceleration is computed: 1 + 𝑓 ̂ 𝑓 ̂ 𝑚1 + 𝑚2 An error termination will occur if a rigid body node is used in a spring definition where compression is limited. 𝑎 ̂common = (19.19) . 19.4 Linear Elastic or Linear Viscous These discrete elements have the simplest force-displacement relations. The linear elastic discrete element has a force-displacement relation of the form 𝑓 ̂ = 𝐾Δ𝑙, (19.20) where 𝐾 is the element’s stiffness and Δ𝑙 is the change in length of the element. The linear viscous element has a similar force-velocity (rate of displacement) relation: where 𝐶 is a viscous damping parameter and Δ𝑡 is the time step increment. 𝑓 ̂ = 𝐶 Δ𝑙 Δ𝑡 . (19.21) 19.5 Nonlinear Elastic or Nonlinear Viscous These discrete elements use piecewise force-displacement or force-relative velocity relations. The nonlinear elastic discrete element has a tabulated force- displacement relation of the form 𝑓 ̂ = 𝐾Δ𝑙, (19.22) where 𝐾(Δ𝑙) is the tabulated force that depends on the total change in the length of the element (Figure 19.1) The nonlinear viscous element has a similar tabulated force- relative velocity relation: 𝑓 ̂ = 𝐶 Δ𝑙 Δ𝑡 , (19.23) where 𝐶(Δ𝑙 element’s length. Nonlinear discrete elements unload along the loading paths. Δ𝑡) is the viscous damping force that depends on the rate of change of the If the spring element is initially of zero length and if no orientation vectors are used then only the tensile part of the stress strain curve needs to be defined. However, Discrete Elements and Masses LS-DYNA Theory Manual Nolinear Elastic/Viscous Displacement/Velocity Figure 19.1. Piecewise linear force-displacement curve for nonlinear elastic discrete element. if the spring element is initially of finite length then the curve must be defined in both the positive and negative quadrants. 19.6 Elasto-Plastic with Isotropic Hardening The elasto-plastic discrete element has a bilinear force-displacement relationship that is specified by the elastic stiffness, a tangent stiffness and a yield force (Figure 19.2). This discrete element uses the elastic stiffness model for unloading until the yield force is exceeded during unloading. The yield force is updated to track its maximum value which is equivalent to an isotropic hardening model. The force-displacement relation during loading may be written as 𝑓 ̂ = 𝐹𝑦 (1 − 𝐾𝑡 ) + 𝐾𝑡Δ𝑙, (19.24) where 𝐹𝑦 is the yield force and 𝐾𝑡 is the tangent stiffness. 19.7 General Nonlinear The general nonlinear discrete element allows the user to specify independent and nonsymmetrical piecewise linear loading and unloading paths (Figure 19.3(a)). LS-DYNA Theory Manual Discrete Elements and Masses Elsto-Plastic with Isotropic Hardening ET FY Elasto-Plastic Unloading Figure 19.2. Loading and unloading force-displacement curves for elasto- plastic discrete element. Displacement This element combines the features of the above-described nonlinear elastic and elasto-plastic discrete elements by allowing the user to specify independent initial yield forces in tension (FYT) and in compression (FYC). If the discrete element force remains between these initial yield values, the element unloads along the loading path (Figure 19.3(b)). This corresponds to the nonlinear elastic discrete element. However, if the discrete element force exceeds either of these initial yield values, the specified unloading curve is used for subsequent unloading. Additionally, the initial loading and unloading curves are allowed to move in the force-displacement space by specifying a mixed hardening parameter 𝛽, where 𝛽 = 0 corresponds to kinematic hardening (Figure 19.3(c)) and 𝛽 = 0 𝛽 = 1 corresponds to isotropic hardening (Figure 19.3(d)). 19.8 Linear Visco-Elastic The linear viscoelastic discrete element [Schwer, Cheva, and Hallquist 1991] allows the user to model discrete components that are characterized by force relaxation or displacement creep behavior. The element’s variable stiffness is defined by three parameters and has the form 𝐾(𝑡) = 𝐾∞ + (𝐾0 − 𝐾∞)𝑒−𝛽𝑡, (19.25) Discrete Elements and Masses LS-DYNA Theory Manual loading curve options β>0 β=0 yt - F yc Fyt Fyc β>0 β=0 unloading curve kinematic hardening β<1 isotropic hardening β=1 force force Fyt-Fyc F2 F2 F1 Figure 19.3. Loading and unloading force displacement curves for general nonlinear discrete element. where 𝐾∞ is the long duration stiffness, 𝐾0 is the short time stiffness, and 𝛽 is a decay parameter that controls the rate at which the stiffness transitions between the short and long duration stiffness (Figure 16.4). This model corresponds to a three-parameter Maxwell model which consists of a spring and damper in series connected to another spring in parallel. Although this discrete element behavior could be built up using the above- described linear elastic and linear viscous discrete elements, such a model would also require the user to specify the nodal mass at the connection of the series spring and damper. This mass introduces a fourth parameter which would further complicate fitting the model to experimental data. LS-DYNA Theory Manual Discrete Elements and Masses Log K0 ) ( Log K∞ K∞ Visco-Elastic K0-K∞ 1/β Log t Figure 19.4. Typical stiffness relaxation curve used for the viscoelastic discrete element. 19.9 Muscle Model This is Material Type 15 for discrete springs and dampers. This material is a Hill-type muscle model with activation. It is for use with discrete elements. The LS- DYNA implementation is due to Dr. J.A. Weiss. L0 VMAX SV Initial muscle length, Lo. Maximum CE shortening velocity, Vmax. Scale factor, Sv, for Vmax vs. active state. A Activation level vs. time function. LT.0: absolute value gives load curve ID GE.0: constant value of 1.0 is used LT.0: absolute value gives load curve ID GE.0: constant value of A is used FMAX Peak isometric force, Fmax. TL Active tension vs. length function. LT.0: absolute value gives load curve ID GE.0: constant value of 1.0 is used Discrete Elements and Masses LS-DYNA Theory Manual FM FCE FPE a(t) SEE LM vM CE LM PE FM Figure 19.5. Discrete model for muscle contraction dynamics, based on a Hill- type representation. The total force is the sum of passive force FPE and active force FCE. The passive element (PE) represents energy storage from muscle elasticity, while the contractile element (CE) represents force generation by the muscle. The series elastic element (SEE), shown in dashed lines, is often neglected when a series tendon compliance is included. Here, a(t) is the activation level, LM is the length of the muscle, and vM is the shortening velocity of the muscle. TV Active tension vs. velocity function. FPE Force vs. length function, Fpe, for parallel elastic element. LT.0: absolute value gives load curve ID GE.0: constant value of 1.0 is used LT.0: absolute value gives load curve ID EQ.0: exponential function is used GT.0: constant value of 0.0 is used Relative length when Fpe reaches Fmax. Required if Fpe = 0 above. LMAX KSH Constant, Ksh, governing the exponential rise of Fpe. Required if Fpe = 0 above. The material behavior of the muscle model is adapted from the original model proposed by Hill (1938). Reviews of this model and extensions can be found in Winters (1990) and Zajac (1989). The most basic Hill-type muscle model consists of a contractile element (CE) and a parallel elastic element (PE) (Figure 19.5). An additional series elastic element (SEE) can be added to represent tendon compliance. The main assumptions of the Hill model are that the contractile element is entirely stress free and freely distensible in the resting state, and is described exactly by Hill’s equation (or some variation). When the muscle is activated, the series and parallel elements are elastic, and the whole muscle is a simple combination of identical sarcomeres in series and parallel. The main criticism of Hill’s model is that the division of forces between the parallel elements and the division of extensions between the series elements is arbitrary, and cannot be made without introducing auxiliary hypotheses. However, these criticisms apply to any discrete element model. Despite these limitations, the Hill model has become extremely useful for modeling musculoskeletal dynamics, as illustrated by its widespread use today. When the contractile element (CE) of the Hill model is inactive, the entire resistance to elongation is provided by the PE element and the tendon load-elongation LS-DYNA Theory Manual Discrete Elements and Masses behavior. As activation is increased, force then passes through the CE side of the parallel Hill model, providing the contractile dynamics. The original Hill model accommodated only full activation - this limitation is circumvented in the present implementation by using the modification suggested by Winters (1990). The main features of his approach were to realize that the CE force-velocity input force equals the CE tension-length output force. This yields a three-dimensional curve to describe the force-velocity-length relationship of the CE. If the force-velocity y-intercept scales with activation, then given the activation, length and velocity, the CE force can be determined. Without the SEE, the total force in the muscle FM is the sum of the force in the CE and the PE because they are in parallel: 𝐹M = 𝐹PE + 𝐹CE. (19.26) The relationships defining the force generated by the CE and PE as a function of LM, VM and 𝑎(𝑡) are often scaled by 𝐹max, the peak isometric force (p. 80, Winters 1990), L0, the initial length of the muscle (p. 81, Winters 1990), and 𝑉max, the maximum unloaded CE shortening velocity (p. 80, Winters 1990). From these, dimensionless length and velocity can be defined: 𝐿 = 𝑉 = 𝐿M 𝐿o , 𝑉M 𝑉max ∗ 𝑆V(𝑎(t)) . (19.27) Here, 𝑆V scales the maximum CE shortening velocity 𝑉max and changes with activation level 𝑎(𝑡). This has been suggested by several researchers, i.e. Winters and Stark [1985]. The activation level specifies the level of muscle stimulation as a function of time. Both have values between 0 and 1. The functions 𝑆V(𝑎(𝑡)) and 𝑎(𝑡) are specified via load curves in LS-DYNA, or default values of 𝑆V = 1 and 𝑎(𝑡) = 0 are used. Note that L is always positive and that 𝑉 is positive for lengthening and negative for shortening. The relationship between FCE, V and L was proposed by Bahler et al. [1967]. A three-dimensional relationship between these quantities is now considered standard for computer implementations of Hill-type muscle models [i.e., eqn 5.16, p. 81, Winters 1990]. It can be written in dimensionless form as: 𝐹CE = 𝑎(𝑡) ∗ 𝐹max ∗ 𝑓TL(𝐿) ∗ 𝑓TV(𝑉), (19.28) The force in the parallel elastic element FPE is determined directly from the current length of the muscle using an exponential relationship [eqn 5.5, p. 73, Winters 1990]: 𝑓PE = 𝐹PE 𝐹MAX = 0 𝐿 ≤ 1 𝑓PE = 𝐹PE 𝐹MAX = exp(𝐾sh) − 1 [exp ⎜⎛ 𝐾sh 𝐿max ⎝ (L − 1) ⎟⎞ − 1] 𝐿 > 1 ⎠ (19.29) Discrete Elements and Masses LS-DYNA Theory Manual Figure 19.6. Typical normalized tension-length (TL) and tension-velocity (TV) curves for skeletal muscle. For computation of the total force developed in the muscle FM, the functions for the tension-length 𝑓TLand force-velocity 𝑓TV relationships used in the Hill element must be defined. These relationships have been available for over 50 years, but have been refined to allow for behavior such as active lengthening. The active tension-length curve 𝑓TL describes the fact that isometric muscle force development is a function of length, with the maximum force occurring at an optimal length. According to Winters, this optimal length is typically around 𝐿 = 1.05, and the force drops off for shorter or longer lengths, approaching zero force for 𝐿 = 0.4 and 𝐿 = 1.5. Thus the curve has a bell-shape. Because of the variability in this curve between muscles, the user must specify the function 𝑓TL via a load curve, specifying pairs of points representing the normalized force (with values between 0 and 1) and normalized length 𝐿 (Figure 19.6). The active tension-velocity relationship 𝑓TV used in the muscle model is mainly due to the original work of Hill. Note that the dimensionless velocity V is used. When V = 0, the normalized tension is typically chosen to have a value of 1.0. When V is greater than or equal to 0, muscle lengthening occurs. As V increases, the function is typically designed so that the force increases from a value of 1.0 and asymptotes towards a value near 1.4. When V is less than zero, muscle shortening occurs and the classic Hill equation hyperbola is used to drop the normalized tension to 0 (Figure 16.6). The user must specify the function 𝑓TV via a load curve, specifying pairs of points representing the normalized tension (with values between 0 and 1) and normalized velocity V. LS-DYNA Theory Manual Discrete Elements and Masses 19.10 Seat Belt Material The seat belt capability reported here was developed by Walker and co-workers [Walker and Dallard 1991, Strut, Walker, et al., 1991] and this section excerpted from their documentation. Each belt material defines stretch characteristics and mass properties for a set of belt elements. The user enters a load curve for loading, the points of which are (Strain, Force). Strain is defined as engineering strain, i.e. Strain = current length initial length − 1. (19.30) Another similar curve is entered to describe the unloading behavior. Both loadcurves should start at the origin (0,0) and contain positive force and strain values only. The belt material is tension only with zero forces being generated whenever the strain becomes negative. The first non-zero point on the loading curve defines the initial yield point of the material. On unloading, the unloading curve is shifted along the strain axis until it crosses the loading curve at the ‘yield’ point from which unloading commences. If the initial yield has not yet been exceeded or if the origin of the (shifted) unloading curve is at negative strain, the original loading curves will be used for both loading and unloading. If the strain is less than the strain at the origin of the unloading curve, the belt is slack and no force is generated. Otherwise, forces will then be determined by the unloading curve for unloading and reloading until the strain again exceeds yield after which the loading curves will again be used. A small amount of damping is automatically included. This reduces high frequency oscillation, but, with realistic force-strain input characteristics and loading rates, does not significantly alter the overall forces-strain performance. The damping forced opposes the relative motion of the nodes and is limited by stability: 𝐷 = . 1 × mass × relative velocity timestep size . (19.31) In addition, the magnitude of the damping forces is limited to one tenth of the force calculated from the forces-strain relationship and is zero when the belt is slack. Damping forces are not applied to elements attached to sliprings and retractors. The user inputs a mass per unit length that is used to calculate nodal masses on initialization. A ‘minimum length’ is also input. This controls the shortest length allowed in any element and determines when an element passes through sliprings or are absorbed into the retractors. One tenth of a typical initial element length is usually a good choice. Discrete Elements and Masses LS-DYNA Theory Manual 19.11 Seat Belt Elements Belt elements are single degree of freedom elements connecting two nodes and are treated in a manner similar to the spring elements. When the strain in an element is positive (i.e., the current length is greater then the unstretched length), a tension force is calculated from the material characteristics and is applied along the current axis of the element to oppose further stretching. The unstretched length of the belt is taken as the initial distance between the two nodes defining the position of the element plus the initial slack length. At the beginning of the calculation the seatbelt elements can be obtained within a retractor. 19.12 Sliprings Sliprings are defined in the LS-DYNA input by giving a slipring ID and element ID’s for two elements who share a node which is coincident with the slipring node. The slipring node may not be attached to any belt elements. Sliprings allow continuous sliding of a belt through a sharp change of angle. Two elements (1 and 2 in Figure 19.7) meet at the slipring. Node B in the belt material remains attached to the slipring node, but belt material (in the form of unstretched length) is passed from element 1 to element 2 to achieve slip. The amount of slip at each timestep is calculated from the ratio of forces in elements 1 and 2. The ratio of forces is determined by the relative angle between elements 1 and 2 and the coefficient of friction, 𝜇. The tension in the belts is taken as T1 and T2, where T2 is on the high- tension side and T1 is the force on the low-tension side. Thus if T2 is sufficiently close to T1 no slip occurs; otherwise, slip is just sufficient to reduce the ratio T2⁄T1 to 𝑒𝜇𝜃. No slip occurs if both elements are slack. The out-of-balance force at node B is reacted on the slipring node; the motion of node B follows that of slipring node. If, due to slip through the slipring, the unstretched length of an element becomes less than the minimum length (as entered on the belt material card), the belt is remeshed locally: the short element passes through the slipring and reappears on the other side . The new unstretched length of e1 is 1.1 × minimum length. Force and strain in e2 and e3 are unchanged; force and strain in e1 are now equal to those in e2. Subsequent slip will pass material from e3 to e1. This process can continue with several elements passing in turn through the slipring. To define a slipring, the user identifies the two belt elements which meet at the slipring, the friction coefficient, and the slipring node. The two elements must have a common node coincident with the slipring node. No attempt should be made to restrain or constrain the common node for its motion will automatically be constrained to follow the slipring node. Typically, the slipring node is part of the vehicle body LS-DYNA Theory Manual Discrete Elements and Masses Slip ring Element 2 Element 1 Element 1 Element 3 Element 2 Element 3 Before After Figure 19.7. Elements passing through slipring. structure and, therefore, belt elements should not be connected to this node directly, but any other feature can be attached, including rigid bodies. 19.13 Retractors Retractors are defined by giving a node, the “retractor node” and an element ID of an element outside the retractor but with one node that is coincident with the retractor node. Also sensor ID’s must be defined for up to four sensors which can activate the seatbelt. Retractors allow belt material to be paid out into a belt element, and they operate in one of two regimes: unlocked when the belt material is paid out or reeled in under constant tension and locked when a user defined force-pullout relationship applies. The retractor is initially unlocked, and the following sequence of events must occur for it to become locked: • Any one of up to four sensors must be triggered. (The sensors are described below). • Then a user-defined time delay occurs. • Then a user-defined length of belt must be payed out (optional). • Then the retractor locks. and once locked, it remains locked. Discrete Elements and Masses LS-DYNA Theory Manual In the unlocked regime, the retractor attempts to apply a constant tension to the belt. This feature allows an initial tightening of the belt, and takes up any slack whenever it occurs. The tension value is taken from the first point on the force-pullout load curve. The maximum rate of pull out or pull in is given by 0.01 × fed length per time step. Because of this, the constant tension value is not always achieved. In the locked regime, a user-defined curve describes the relationship between the force in the attached element and the amount of belt material paid out. If the tension in the belt subsequently relaxes, a different user-defined curve applies for unloading. The unloading curve is followed until the minimum tension is reached. The curves are defined in terms of initial length of belt. For example, if a belt is marked at 10mm intervals and then wound onto a retractor, and the force required to make each mark emerge from the (locked) retractor is recorded, the curves used for input would be as follows: 0 Minimum tension (should be > zero) 10 mm Force to emergence of first mark 20 mm Force to emergence of second mark .. .. .. Pyrotechnic pretensions may be defined which cause the retractor to pull in the belt at a predetermined rate. This overrides the retractor force-pullout relationship from the moment when the pretensioner activates. If desired, belt elements may be defined which are initially inside the retractor. These will emerge as belt material is paid out, and may return into the retractor if sufficient material is reeled in during unloading. Elements e2, e3 and e4 are initially inside the retractor, which is paying out material into element e1. When the retractor has fed Lcrit into e1, where: Lcrit = fed length − 1.1 × minimum length (19.32) Here, minimum length is defined on belt material input, and fed length is defined on retractor input. element e2 emerges with an unstretched length of 1.1 × minimum length; the unstretched length of element e1 is reduced by the same amount. The force and strain in e1 are unchanged; in e2, they are set equal to those in e1. The retractor now pays out material into e2. LS-DYNA Theory Manual Discrete Elements and Masses If no elements are inside the retractor, e2 can continue to extend as more material is fed into it. As the retractor pulls in the belt (for example, during initial tightening), if the unstretched length of the mouth element becomes less than the minimum length, the element is taken into the retractor. To define a retractor, the user enters the retractor node, the ‘mouth’ element (into which belt material will be fed, e1 in Figure 19.8, up to 4 sensors which can trigger unlocking, a time delay, a payout delay (optional), load and unload curve numbers, and the fed length. The retractor node is typically part of the vehicle stricture; belt elements should not be connected to this node directly, but any other feature can be attached including rigid bodies. The mouth element should have a node coincident with the retractor but should not be inside the retractor. The fed length would typically be set either to a typical element initial length, for the distance between painted marks on a real belt for comparisons with high-speed film. The fed length should be at least three times the minimum length. If there are elements initially inside the retractor (e2, e3 and e4 in the Figure) they should not be referred to on the retractor input, but the retractor should be identified on the element input for these elements. Their nodes should all be coincident with the retractor node and should not be restrained or constrained. Initial slack will automatically be set to 1.1 × minimum length for these elements; this overrides any user-defined value. Discrete Elements and Masses LS-DYNA Theory Manual Before Element 1 Element 1 Element 2 Element 4 Element 3 Element 2 After Element 3 Element 4 Element 4 Element 4 All nodes within this area are coincident Figure 19.8. Elements in a retractor. Weblockers can be included within the retractor representation simply by entering a ‘locking up’ characteristic in the force pullout curve, see Figure 19.9. The final section can be very steep (but must have a finite slope). with weblockers without weblockers Pullout Figure 19.9. Retractor force pull characteristics. LS-DYNA Theory Manual Discrete Elements and Masses 19.14 Sensors Sensors are used to trigger locking of retractors and activate pretensioners. Four types of sensor are available which trigger according to the following criteria: Type 1–When the magnitude of x-, y-, or z- acceleration of a given node has remained above a given level continuously for a given time, the sensor triggers. This does not work with nodes on rigid bodies. Type 2–When the rate of belt payout from a given retractor has remained above a given level continuously for a given time, the sensor triggers. Type 3–The sensor triggers at a given time. Type 4–The sensor triggers when the distance between two nodes exceeds a given maximum or becomes less than a given minimum. This type of sensor is intended for use with an explicit mas/spring representation of the sensor mechanism. By default, the sensors are inactive during dynamic relaxation. This allows initial tightening of the belt and positioning of the occupant on the seat without locking the retractor or firing any pretensioners. However, a flag can be set in the sensor input to make the sensors active during the dynamic relaxation phase. 19.15 Pretensioners Pretensioners allow modeling of three types of active devices which tighten the belt during the initial stages of a crash. The first type represents a pyrotechnic device which spins the spool of a retractor, causing the belt to be reeled in. The user defines a pull-in versus time curve which applies once the pretensioner activates. The remaining types represents preloaded springs or torsion bars which move the buckle when released. The pretensioner is associated with any type of spring element including rotational. Note that the preloaded spring, locking spring and any restraints on the motion of the associated nodes are defined in the normal way; the action of the pretensioner is merely to cancel the force in one spring until (or after) it fires. With the second type, the force in the spring element is cancelled out until the pretensioner is activated. In this case the spring in question is normally a stiff, linear spring which acts as a locking mechanism, preventing motion of the seat belt buckle relative to the vehicle. A preloaded spring is defined in parallel with the locking spring. This type avoids the problem of the buckle being free to ‘drift’ before the pretensioner is activated. To activate the pretensioner the following sequence of events must occur: Discrete Elements and Masses LS-DYNA Theory Manual 1. Any one of up to four sensors must be triggered. 2. Then a user-defined time delay occurs. 3. Then the pretensioner acts. 19.16 Accelerometers The accelerometer is defined by three nodes in a rigid body which defines a triad to measure the accelerations in a local system. The presence of the accelerometer means that the accelerations and velocities of node 1 will be output to all output files in local instead of global coordinates. The local coordinate system is defined by the three nodes as follows: • local 𝐱 from node 1 to node 2 • local 𝐳 perpendicular to the plane containing nodes, 1, 2, and 3 (𝐳 = 𝐱 × 𝐚), where 𝐚 is from node 1 to node 3). • local 𝐲 = 𝐱 × 𝐳 The three nodes should all be part of the same rigid body. The local axis then rotates with the body. LS-DYNA Theory Manual Simplified Arbitrary Lagrangian-Eulerian 20 Simplified Arbitrary Lagrangian- Eulerian Arbitrary Lagrangian-Eulerian (ALE) formulations may be thought of as algorithms that perform automatic rezoning. Users perform manual rezoning by 1. 2. Stopping the calculation when the mesh is distorted, Smoothing the mesh, 3. Remapping the solution from the distorted mesh to the smooth mesh. An ALE formulation consists of a Lagrangian time step followed by a “remap” or “advection” step. The advection step performs an incremental rezone, where “incremental” refers to the fact that the positions of the nodes are moved only a small fraction of the characteristic lengths of the surrounding elements. Unlike a manual rezone, the topology of the mesh is fixed in an ALE calculation. An ALE calculation can be interrupted like an ordinary Lagrangian calculation and a manual rezone can be performed if an entirely new mesh is necessary to continue the calculation. The accuracy of an ALE calculation is often superior to the accuracy of a manually rezoned calculation because the algorithm used to remap the solution from the distorted to the undistorted mesh is second order accurate for the ALE formulation while the algorithm for the manual rezone is only first order accurate. In theory, an ALE formulation contains the Eulerian formulation as a subset. Eulerian codes can have more than one material in each element, but most ALE implementations are simplified ALE formulations which permit only a single material in each element. The primary advantage of a simplified formulation is its reduced cost per time step. When elements with more than one material are permitted, the number and types of materials present in an element can change dynamically. Additional data Simplified Arbitrary Lagrangian-Eulerian LS-DYNA Theory Manual is necessary to specify the materials in each element and the data must be updated by the remap algorithms. The range of problems that can be solved with an ALE formulation is a direct function of the sophistication of the algorithms for smoothing the mesh. Early ALE codes were not very successful largely because of their primitive algorithms for smoothing the mesh. In simplified ALE formulations, most of the difficulties with the mesh are associated with the nodes on the material boundaries. If the material boundaries are purely Lagrangian, i.e., the boundary nodes move with the material at all times, no smooth mesh maybe possible and the calculation will terminate. The algorithms for maintaining a smooth boundary mesh are therefore as important to the robustness of the calculations as the algorithms for the mesh interior. The cost of the advection step per element is usually much larger than the cost of the Lagrangian step. Most of the time in the advection step is spent in calculating the material transported between the adjacent elements, and only a small part of it is spent on calculating how and where the mesh should be adjusted. Second order accurate monotonic advection algorithms are used in LS-DYNA despite their high cost per element because their superior coarse mesh accuracy which allows the calculation to be performed with far fewer elements than would be possible with a cheaper first order accurate algorithm. The second order transport accuracy is important since errors in the transport calculations generally smooth out the solution and reduce the peak values in the history variables. Monotonic advection algorithms are constructed to prevent the transport calculations from creating new minimum or maximum values for the solution variables. They were first developed for the solution of the Navier Stokes equations to eliminate the spurious oscillations that appeared around the shock fronts. Although monotonic algorithms are more diffusive than algorithms that are not monotonic, they must be used for stability in general purpose codes. Many constitutive models have history variables that have limited ranges, and if their values are allowed to fall outside of their allowable ranges, the constitutive models are undefined. Examples include explosive models, which require the burn fraction to be between zero and one, and many elastoplasticity models, such as those with power law hardening, which require a non- negative plastic strain. The overall flow of an ALE time step is: 1. 2. Perform a Lagrangian time step. Perform an advection step. a) Decide which nodes to move. b) Move the boundary nodes. LS-DYNA Theory Manual Simplified Arbitrary Lagrangian-Eulerian c) Move the interior nodes. d) Calculate the transport of the element-centered variables. e) Calculate the momentum transport and update the velocity. Each element solution variable must be transported. The total number of solution variables, including the velocity, is at least six and depends on the material models. For elements that are modeled with an equation of state, only the density, the internal energy, and the shock viscosity are transported. When the elements have strength, the six components of the stress tensor and the plastic strain must also be advected, for a total of ten solution variables. Kinematic hardening, if it is used, introduces another five solution variables, for a total of fifteen. The nodal velocities add an extra three solution variables that must be transported, and they must be advected separately from the other solution variables because they are centered at the nodes and not in the elements. In addition, the momentum must be conserved, and it is a product of the node-centered velocity and the element-centered density. This imposes a constraint on how the momentum transport is performed that is unique to the velocity field. A detailed consideration of the difficulties associated with the transport of momentum is deferred until later. Perhaps the simplest strategy for minimizing the cost of the ALE calculations is to perform them only every few time steps. The cost of an advection step is typically two to five times the cost of the Lagrangian time step. By performing the advection step only every ten steps, the cost of an ALE calculation can often be reduced by a factor of three without adversely affecting the time step size. In general, it is not worthwhile to advect an element unless at least twenty percent of its volume will be transported because the gain in the time step size will not offset the cost of the advection calculations. 20.1 Mesh Smoothing Algorithms The algorithms for moving the mesh relative to the material control the range of the problems that can be solved by an ALE formulation. The equipotential method which is used in LS-DYNA was developed by Winslow [1990] and is also used in the DYNA2D ALE code [Winslow 1963]. It, and its extensions, have proven to be very successful in a wide variety of problems. The following is extracted from reports prepared by Alan Winslow for LSTC. Simplified Arbitrary Lagrangian-Eulerian LS-DYNA Theory Manual 20.1.1 Equipotential Smoothing of Interior Nodes “Equipotential” zoning [Winslow, 1963] is a method of making a structured mesh for finite difference or finite element calculations by using the solutions of Laplace equations (later extended to Poisson equations) as the mesh lines. The same method can be used to smooth selected points in an unstructured three-dimensional mesh provided that it is at least locally structured. This chapter presents a derivation of the three-dimensional equipotential zoning equations, taken from the references, and gives their finite difference equivalents in a form ready to be used for smoothing interior points. We begin by reviewing the well-known two-dimensional zoning equations, and then discuss their extension to three dimensions. In two dimensions we define curvilinear coordinates 𝜉 𝜂 which satisfy Laplace’s equation: ∇2𝜉 = 0, ∇2𝜂 = 0. (20.1.1a) (1.1.1b) We solve Equations (1.1.1b) for the coordinates 𝑥(𝜉 , 𝜂) and 𝑦(𝜉 , 𝜂) of the mesh lines: that is, we invert them so that the geometric coordinates 𝑥, 𝑦 become the dependent variables and the curvilinear coordinates 𝜉 , 𝜂 the independent variables. By the usual methods of changing variables we obtain 𝛼𝑥𝜉𝜉 − 2𝛽𝑥𝜉𝜂 + 𝛾𝑥𝜂𝜂 = 0, 𝛼𝑦𝜉𝜉 − 2𝛽𝑦𝜉𝜂 + 𝛾𝑦𝜂𝜂 = 0, where 𝛼 ≡ 𝑥𝜂 2 + 𝑦𝜂 2, 𝛽 ≡ 𝑥𝜉 𝑥𝜂 + 𝑦𝜉 𝑦𝜂, 𝛾 ≡ 𝑥𝜉 2. 2 + 𝑦𝜉 Equations (16.1.2) can be written in vector form: 𝛼𝐫𝜉𝜉 − 2𝛽𝐫𝜉𝜂 + 𝛾𝐫𝜂𝜂 = 𝟎, where 𝐫 ≡ 𝑥𝐢 + 𝑦𝐣. (20.1.2a) (20.1.2b) (20.1.3) (20.1.4) (20.1.5) We differentiate Equations (20.1.4) and solve them numerically by an iterative method, since they are nonlinear. In (𝜉 , 𝜂) space, we use a mesh whose curvilinear coordinates are straight lines which take on integer values corresponding to the usual numbering in a two-dimensional mesh. The numerical solution then gives us the location of the “equipotential” mesh lines. In three dimensions 𝑥, 𝑦, 𝑧, we add a third curvilinear coordinate 𝜁 and a third Laplace equation LS-DYNA Theory Manual Simplified Arbitrary Lagrangian-Eulerian ∇2𝜁 = 0. (20.1.1c) Inversion of the system of three equations (17.1.1) by change of variable is rather complicated. It is easier, as well as more illuminating, to use the methods of tensor analysis pioneered by Warsi [1982]. Let the curvilinear coordinates be represented by 𝜉 𝑖(𝑖 = 1,2,3). For a scalar function 𝐴(𝑥, 𝑦, 𝑧),Warsi shows that the transformation of its Laplacian from rectangular Cartesian to curvilinear coordinates is given by ∇2𝐴 = ∑ 𝑔𝑖𝑗𝐴𝜉 𝑖𝜉 𝑗 + ∑(∇2𝜉 𝑘)𝐴𝜉 𝑘 , (20.1.6) 𝑖,𝑗=1 𝑘=1 where a variable subscript indicates differentiation with respect to that variable. Since the curvilinear coordinates are each assumed to satisfy Laplace’s equation, the second summation in Equation (20.1.6) vanishes and we have ∇2𝐴 = ∑ 𝑔𝑖𝑗𝐴𝜉 𝑖𝜉 𝑗 . 𝑖,𝑗=1 (20.1.7) If now we let 𝐴 = 𝑥, 𝑦, and 𝑧 successively, the left-hand side of (20.1.7) vanishes in each case and we get three equations which we can write in vector form ∑ 𝑔𝑖𝑗𝐫𝜉 𝑖𝜉 𝑗 = 0 . 𝑖,𝑗=1 (20.1.8) Equation (20.1.8) is the three-dimensional generalization of Equations (20.1.4), and it only remains to determine the components of the contravariant metric tensor 𝑔𝑖𝑗 in three dimensions. These are defined to be 𝑔𝑖𝑗 ≡ 𝐚𝑖 ⋅ 𝐚𝑗, (20.1.9) where the contravariant base vectors of the transformation from (𝑥, 𝑦, 𝑧) to (𝜉 1, 𝜉 2, 𝜉 3) are given by 𝐚𝑖 ≡ ∇𝜉 𝑖 = 𝐚𝑗 × 𝐚𝑘 √𝑔 , (20.1.10) (𝑖, 𝑗, 𝑘 cyclic). Here the covariant base vectors, the coordinate derivatives, are given by 𝐚𝑖 ≡ 𝐫𝜉 𝑖, 𝐫 ≡ 𝑥ı̂ + 𝑦ĵ + 𝑧𝐤̂ . where Also, 𝑔 ≡ det(𝑔𝑖𝑗) = [𝐚1 ⋅ (𝐚2 × 𝐚3)]2 = 𝐽2, (20.1.11) (20.1.12) (20.1.13) Simplified Arbitrary Lagrangian-Eulerian LS-DYNA Theory Manual where 𝑔𝑖𝑗 is the covariant metric tensor given by 𝑔𝑖𝑗 ≡ 𝐚𝑖 ⋅ 𝐚𝑗, (20.1.14) and 𝐽 is the Jacobian of the transformation. Substituting (20.1.10) into (20.1.9), and using the vector identity (𝐚 × 𝐛) ⋅ (𝐜 × 𝐝) ≡ (𝐚 ⋅ 𝐜) ⋅ (𝐛 ⋅ 𝐝) − (𝐚 ⋅ 𝐝)(𝐛 ⋅ 𝐜), (20.1.15) we get 𝑔𝑔𝑖𝑖 = 𝐚𝑗 2𝐚𝑘 2 − (𝐚𝑗 ⋅ 𝐚𝑘) = 𝑔𝑗𝑗𝑔𝑘𝑘 − (𝑔𝑗𝑘) , 𝑔𝑔𝑖𝑗 = (𝐚𝑖 ⋅ 𝐚𝑘)(𝐚𝑗 ⋅ 𝐚𝑘) − (𝐚𝑖 ⋅ 𝐚𝑗)𝐚𝑘 2 = 𝑔𝑖𝑘𝑔𝑗𝑘 − 𝑔𝑖𝑗𝑔𝑘𝑘. (20.1.16) (20.1.17) Before substituting (20.1.11) into (17.1.13a, b), we return to our original notation: Then, using (20.1.11), we get 𝜉 + 𝜉 1, 𝜂 + 𝜉 2, 𝜁 + 𝜉 3. 𝑔𝑔11 = 𝐫𝜂 2𝐫𝜁 2 − (𝐫𝜂 ⋅ 𝐫𝜁 ) 𝑔𝑔22 = 𝐫𝜁 2𝐫𝜉 2 − (𝐫𝜁 ⋅ 𝐫𝜉 ) 𝑔𝑔33 = 𝐫𝜉 2𝐫𝜂 2 − (𝐫𝜉 ⋅ 𝐫𝜂) , , , for the three diagonal components, and 2, 𝑔𝑔12 = (𝐫𝜉 ⋅ 𝐫𝜁 )(𝐫𝜂 ⋅ 𝐫𝜁 ) − (𝐫𝜉 ⋅ 𝐫𝜂)𝐫𝜁 2, 𝑔𝑔23 = (𝐫𝜂 ⋅ 𝐫𝜉 )(𝐫𝜁 ⋅ 𝐫𝜉 ) − (𝐫𝜂 ⋅ 𝐫𝜁 )𝐫𝜉 2, 𝑔𝑔31 = (𝐫𝜁 ⋅ 𝐫𝜂)(𝐫𝜉 ⋅ 𝐫𝜂) − (𝐫𝜁 ⋅ 𝐫𝜉 )𝐫𝜂 (20.1.18) (20.1.19) (20.1.20) (20.1.21) (20.1.22) (20.1.23) (20.1.24) for the three off-diagonal components of this symmetric tensor. When we express Equations (17.1.15) in terms of the Cartesian coordinates, some cancellation takes place and we can write them in the form 𝑔𝑔11 = (𝑥𝜂𝑦𝜁 − 𝑥𝜁 𝑦𝜂)2 + (𝑥𝜂𝑧𝜁 − 𝑥𝜁 𝑧𝜂)2 + (𝑦𝜂𝑧𝜁 − 𝑦𝜁 𝑧𝜂)2, 𝑔𝑔22 = (𝑥𝜁 𝑦𝜉 − 𝑥𝜉 𝑦𝜁 )2 + (𝑥𝜁 𝑧𝜉 − 𝑥𝜉 𝑧𝜁 )2 + (𝑦𝜁 𝑧𝜉 − 𝑦𝜉 𝑧𝜁 )2, 𝑔𝑔33 = (𝑥𝜉 𝑦𝜂 − 𝑥𝜂𝑦𝜉 )2 + (𝑥𝜉 𝑧𝜂 − 𝑥𝜂𝑧𝜉 )2 + (𝑦𝜉 𝑧𝜂 − 𝑦𝜂𝑧𝜉 )2, (20.1.25) (20.1.26) (20.1.27) guaranteeing positivity as required by Equations (20.1.9). Writing out Equations (17.1.16) we get LS-DYNA Theory Manual Simplified Arbitrary Lagrangian-Eulerian 𝑔𝑔12 = (𝑥𝜉 𝑥𝜁 + 𝑦𝜉 𝑦𝜁 + 𝑧𝜉 𝑧𝜁 )(𝑥𝜂𝑥𝜁 + 𝑦𝜂𝑦𝜁 + 𝑧𝜂𝑧𝜁 ) −(𝑥𝜉 𝑥𝜂 + 𝑦𝜉 𝑦𝜂 + 𝑧𝜉 𝑧𝜂)(𝑥𝜁 2 + 𝑦𝜁 2 + 𝑧𝜁 2), 𝑔𝑔23 = (𝑥𝜂𝑥𝜉 + 𝑦𝜂𝑦𝜉 + 𝑧𝜂𝑧𝜉 )(𝑥𝜁 𝑥𝜉 + 𝑦𝜁 𝑦𝜉 + 𝑧𝜁 𝑧𝜉 ) −(𝑥𝜂𝑥𝜁 + 𝑦𝜂𝑦𝜁 + 𝑧𝜂𝑧𝜁 )(𝑥𝜉 2 + 𝑦𝜉 2 + 𝑧𝜉 2), 𝑔𝑔31 = (𝑥𝜁 𝑥𝜂 + 𝑦𝜁 𝑦𝜂 + 𝑧𝜁 𝑧𝜂)(𝑥𝜉 𝑥𝜂 + 𝑦𝜉 𝑦𝜂 + 𝑧𝜉 𝑧𝜂) −(𝑥𝜁 𝑥𝜉 + 𝑦𝜁 𝑦𝜉 + 𝑧𝜁 𝑧𝜉 )(𝑥𝜂 2 + 𝑦𝜂 2 + 𝑧𝜂 2). (20.1.28) (20.1.29) (20.1.30) Hence, we finally write Equations (20.1.8) in the form 𝑔(𝑔11𝐫𝜉𝜉 + 𝑔22𝐫𝜂𝜂 + 𝑔33𝐫𝜁𝜁 + 2𝑔12𝐫𝜉𝜂 + 2𝑔23𝐫𝜂𝜁 + 2𝑔31𝐫𝜁𝜉 ) = 0, (20.1.31) where the 𝑔𝑔𝑖𝑗 are given by Equations (17.1.17) and (17.1.18). Because Equations (20.1.8) are homogeneous, we can use 𝑔𝑔𝑖𝑗 in place of 𝑔𝑖𝑗 as long as 𝑔 is positive, as it must be for a nonsingular transformation. We can test for positivity at each mesh point by using Equation (1.1.32): √𝑔 = 𝐽 = 𝑥𝜉 𝑥𝜂 𝑥𝜁 ∣ ∣∣ ∣ 𝑦𝜉 𝑦𝜂 𝑦𝜁 𝑧𝜉 ∣ 𝑧𝜂 ∣∣ , 𝑧𝜁 ∣ (20.1.32) and requiring that 𝐽 > 0. To check that these equations reproduce the two-dimensional equations when there is no variation in one-dimension, we take 𝜁 as the invariant direction, thus reducing (17.1.19) to 𝑔𝑔11𝐫𝜉𝜉 + 2𝑔𝑔12𝐫𝜉𝜂 + 𝑔𝑔22𝐫𝜂𝜂 = 0. If we let 𝜁 = 𝑧, then the covariant base vectors become 𝐚1 = 𝑥𝜉 𝐢 + 𝑦𝜉 𝐣, 𝐚2 = 𝑥𝜂𝐢 + 𝑦𝜂𝐣, 𝐚3 = 𝐤. From (17.1.22), using (17.1.13), we get 𝑔𝑔11 = 𝑥𝜂 2, 2 + 𝑦𝜂 𝑔𝑔22 = 𝑥𝜉 2, 2 + 𝑦𝜉 𝑔𝑔12 = −(𝑥𝜉 𝑥𝜂 + 𝑦𝜉 𝑦𝜂). (20.1.33) (20.1.34) (20.1.35) (20.1.36) (20.1.37) (20.1.38) (20.1.39) Substituting (17.1.23) into (20.1.33) yields the two-dimensional equipotential zoning Equations (17.1.2). Simplified Arbitrary Lagrangian-Eulerian LS-DYNA Theory Manual Before differencing Equations (17.1.19) we simplify the notation and write them in the form where 𝛼1𝐫𝜉𝜉 + 𝛼2𝐫𝜂𝜂 + 𝛼3𝐫𝜁𝜁 + 2𝛽1𝐫𝜉𝜂 + 2𝛽2𝐫𝜂𝜁 + 2𝛽3𝐫𝜁𝜉 = 0, (20.1.40) 𝛼1 = (𝑥𝜂𝑦𝜁 − 𝑥𝜁 𝑦𝜂)2 + (𝑥𝜂𝑧𝜁 − 𝑥𝜁 𝑧𝜂)2 + (𝑦𝜂𝑧𝜁 − 𝑦𝜁 𝑧𝜂)2, 𝛼2 = (𝑥𝜁 𝑦𝜉 − 𝑥𝜉 𝑦𝜁 )2 + (𝑥𝜁 𝑧𝜉 − 𝑥𝜉 𝑧𝜁 )2 + (𝑦𝜁 𝑧𝜉 − 𝑦𝜉 𝑧𝜁 )2, 𝛼3 = (𝑥𝜉 𝑦𝜂 − 𝑥𝜂𝑦𝜉 )2 + (𝑥𝜉 𝑧𝜂 − 𝑥𝜂𝑧𝜉 )2 + (𝑦𝜉 𝑧𝜂 − 𝑦𝜂𝑧𝜉 )2. 𝛽1 = (𝑥𝜉 𝑥𝜁 + 𝑦𝜉 𝑦𝜁 + 𝑧𝜉 𝑧𝜁 )(𝑥𝜂𝑥𝜁 + 𝑦𝜂𝑦𝜁 + 𝑧𝜂𝑧𝜁 ) −(𝑥𝜉 𝑥𝜂 + 𝑦𝜉 𝑦𝜂 + 𝑧𝜉 𝑧𝜂)(𝑥𝜁 2 + 𝑦𝜁 2 + 𝑧𝜁 2), 𝛽2 = (𝑥𝜂𝑥𝜉 + 𝑦𝜂𝑦𝜉 + 𝑧𝜂𝑧𝜉 )(𝑥𝜉 𝑥𝜁 + 𝑦𝜉 𝑦𝜁 + 𝑧𝜉 𝑧𝜁 ) −(𝑥𝜁 𝑥𝜂 + 𝑦𝜁 𝑦𝜂 + 𝑧𝜁 𝑧𝜂)(𝑥𝜉 2 + 𝑦𝜉 2 + 𝑧𝜉 2), 𝛽3 = (𝑥𝜂𝑥𝜁 + 𝑦𝜂𝑦𝜁 + 𝑧𝜂𝑧𝜁 )(𝑥𝜉 𝑥𝜂 + 𝑦𝜉 𝑦𝜂 + 𝑧𝜉 𝑧𝜂) −(𝑥𝜉 𝑥𝜂 + 𝑦𝜉 𝑦𝜂 + 𝑧𝜉 𝑧𝜂)(𝑥𝜂 2 + 𝑦𝜂 2 + 𝑧𝜂 2), (20.1.41) (20.1.42) (20.1.43) (20.1.44) (20.1.45) (20.1.46) We difference Equations (20.1.40) in a cube in the rectangular 𝜉 𝜂 𝜁 space with unit spacing between the coordinate surfaces, using subscript 𝑖 to represent the 𝜉 direction, 𝑗 the 𝜂 direction, and 𝑘 the 𝜁 direction, as shown in Figure 20.1. LS-DYNA Theory Manual Simplified Arbitrary Lagrangian-Eulerian Figure 20.1. Example Caption Using central differencing, we obtain the following finite difference approxima- tions for the coordinate derivatives: 𝐫𝜉 = (𝐫𝑖+1 − 𝐫𝑖−1) 2,⁄ 𝐫𝜂 = (𝐫𝑗+1 − 𝐫𝑗−1) 2⁄ , 𝐫𝜁 = (𝐫𝑘+1 − 𝐫𝑘−1) 2⁄ , 𝐫𝜉𝜉 = (𝐫𝑖+1 − 2𝐫 + 𝐫𝑖−1), 𝐫𝜂𝜂 = (𝐫𝑗+1 − 2𝐫 + 𝐫𝑗−1), 𝐫𝜁𝜁 = (𝐫𝑘+1 − 2𝐫 + 𝐫𝑘−1), 𝐫𝜉𝜂 = [(𝐫𝑖+1,𝑗+1 + 𝐫𝑖−1,𝑗−1) − (𝐫𝑖+1,𝑗−1 + 𝐫𝑖−1,𝑗+1)], 𝐫𝜂𝜁 = 𝐫𝜁𝜉 = [(𝐫𝑗+1,𝑘+1 + 𝐫𝑗−1,𝑘−1) − (𝐫𝑗+1,𝑘−1 + 𝐫𝑗−1,𝑘+1)], [(𝐫𝐼+1,𝑘+1 + 𝐫𝐼−1,𝑘−1) − (𝐫𝐼+1,𝑘−1 + 𝐫𝐼−1,𝑘+1)], (20.1.47) (20.1.48) (20.1.49) (20.1.50) (20.1.51) (20.1.52) (20.1.53) (20.1.54) (20.1.55) where for brevity we have omitted subscripts 𝑖, 𝑗, or 𝑘 (e.g., 𝑘 + 1 stands for 𝑖, 𝑗, 𝑘 + 1). Note that these difference expressions use only coordinate planes that pass through the central point, and therefore do not include the eight corners of the cube. Simplified Arbitrary Lagrangian-Eulerian LS-DYNA Theory Manual Substituting Equations (17.1.26) into (17.1.24,17.1.25) and collecting terms, we get 18 ∑ 𝑚=1 𝜔𝑚(𝐫𝑚 − 𝐫) = 0, (20.1.56) where the sum is over the 18 nearest (in the transform space) neighbors of the given point. The coefficients 𝜔𝑚 are given in Table 17.1. Equations (20.1.56) can be written 𝐫𝑚 = ∑ 𝜔𝑚𝐫𝑚 ∑ ω𝑚𝑚 , (20.1.57) expressing the position of the central point as a weighted mean of its 18 nearest neighbors. The denominator of (20.1.57) is equal to 2(𝛼1 + 𝛼2 + 𝛼3) which is guaranteed to be positive by (17.1.25). This vector equation is equivalent to the three scalar equations (20.1.58) (20.1.59) 𝑥 = ∑ 𝜔𝑚x𝑚 ∑ ω𝑚𝑚 , 𝑦 = ∑ 𝜔𝑚y𝑚 ∑ 𝜔𝑚𝑚 , Index 𝑖 + 1 𝑖– 1 𝑗 + 1 𝑗– 1 𝑘 + 1 𝑘– 1 𝑖 + 1, 𝑗 + 1 𝑖– 1, 𝑗– 1 𝑖 + 1, 𝑗– 1 𝑖– 1, 𝑗 + 1 𝑗 + 1, 𝑘 + 1 𝑗– 1, 𝑘– 1 𝑗 + 1, 𝑘– 1 𝑗– 1, 𝑘 + 1 𝑖 + 1, 𝑘 + 1 𝑖– 1, 𝑘– 1 𝑖 + 1, 𝑘– 1 𝑖– 1, 𝑘 + 1 m 1 2 3 4 5 6 7 8 9 10 11 12 13 14 15 16 17 18 𝜔𝑚 𝛼1 𝛼1 𝛼2 𝛼2 𝛼3 𝛼3 𝛽1/2 𝛽1/2 −𝛽1/2 −𝛽1/2 𝛽2/2 𝛽2/2 −𝛽2/2 −𝛽2/2 𝛽3/2 𝛽3/2 −𝛽3/2 −𝛽3/2 LS-DYNA Theory Manual Simplified Arbitrary Lagrangian-Eulerian Table 17.1. 3D Zoning Weight Coefficients 𝑧 = ∑ 𝜔𝑚𝑧𝑚 ∑ 𝜔𝑚𝑚 . (20.1.60) the same weights 𝜔𝑚 appearing in each equation. These equations are nonlinear, since the coefficients are functions of the coordinates. Therefore we solve them by an iterative scheme, such as SOR. When applied to Equation (20.1.58), for example, this gives for the (n+1)st iteration 𝑥𝑛+1 = (1 − f)𝑥𝑛 + f ( ∑ 𝜔𝑚𝑥𝑚 ∑ 𝜔𝑚𝑚 ), (20.1.61) where the over relaxation factor 𝑓 must satisfy 0 < 𝑓 < 2. In (20.1.61) the values of 𝑥𝑚 at the neighboring points are the latest available values. The coefficients 𝜔𝑚 are recalculated before each iteration using Table 17.1 and Equations (17.1.25). To smooth one interior point in a three-dimensional mesh, let the point to be smoothed be the interior point of Figure 17.1, assuming that its neighborhood has the logical structure shown. Even though Equations (17.1.29) are nonlinear, the 𝜔𝑚 do not involve the coordinates of the central point, since the α’s and β’s do not. Hence we simply solve Equations (17.1.29) for the new coordinates (𝑥, 𝑦, 𝑧), holding the 18 neighboring points fixed, without needing to iterate. If we wish to smooth a group of interior points, we solve iteratively for the coordinates using equations of the form (20.1.61). 20.1.2 Simple Averaging The coordinates of a node is the simple average of the coordinates of its surrounding nodes. 𝑛+1 = 𝑥SA 𝑚tot 𝑚tot ∑ 𝑥𝑚 𝑚=1 . (20.1.62) 20.1.3 Kikuchi’s Algorithm Kikuchi proposed an algorithm that uses a volume-weighted average of the coordinates of the centroids of the elements surrounding a node. Variables that are subscripted with Greek letters refer to element variables, and subscripts with capital letters refer to the local node numbering within an element. n = 𝑥α ∑ 𝑥𝐴 , (20.1.63) Simplified Arbitrary Lagrangian-Eulerian LS-DYNA Theory Manual 𝑛+1 = 𝑥𝐾 αtot ∑ 𝑉a𝑥α α=1 αtot ∑ Va α=1 . (20.1.64) 20.1.4 Surface Smoothing The surfaces are smoothed by extending the two-dimensional equipotential stencils to three dimensions. Notice that the form of Equation (20.1.2a) and (20.1.2b) for the 𝑥 and 𝑦 directions are identical. The third dimension, 𝑧, takes the same form. When Equation (16.1.2) is applied to all three dimensions, it tends to flatten out the surface and alter the total volume. To conserve the volume and retain the curvature of the surface, the point given by the relaxation stencil is projected on to the tangent plane defined by the normal at the node. 20.1.5 Combining Smoothing Algorithms The user has the option of using a weighted average of all three algorithms to generate a composite algorithm, where the subscripts E, SA, and K refer to the equipotential, simple averaging, and Kikuchi’s smoothing algorithm respectively, and ww is the weighting factor. 𝑥𝑛+1 = 𝑤E𝑥E 𝑛+1 + 𝑤SA𝑥SA 𝑛+1 + 𝑤K𝑥K 𝑛+1. (20.1.65) 20.2 Advection Algorithms LS-DYNA follows the SALE3D strategy for calculating the transport of the element-centered variables (i.e., density, internal energy, the stress tensor and the history variables). The van Leer MUSCL scheme [van Leer 1977] is used instead of the donor cell algorithm to calculate the values of the solution variables in the transport fluxes to achieve second order accurate monotonic results. To calculate the momentum transport, two algorithms have been implemented. The less expensive of the two is the one that is implemented in SALE3D, but it has known dispersion problems and may violate monotonocity (i.e., introduce spurious oscillations) [Benson 1992]. As an alternative, a significantly more expensive method [Benson 1992], which can be shown analytically to not have either problem on a regular mesh, has also been implemented. In this section the donor cell and van Leer MUSCL scheme are discussed. Both methods are one-dimensional and their extensions to multidimensional problems are discussed later. 20.2.1 Advection Methods in One Dimension In this section the donor cell and van Leer MUSCL scheme are discussed. Both methods are one-dimensional and their extensions to multidimensional problems are discussed later. LS-DYNA Theory Manual Simplified Arbitrary Lagrangian-Eulerian The remap step maps the solution from a distorted Lagrangian mesh on to the new mesh. The underlying assumptions of the remap step are 1) the topology of the mesh is fixed (a complete rezone does not have this limitation), and 2) the mesh motion during a step is less than the characteristic lengths of the surrounding elements. Within the fluids community, the second condition is simply stated as saying the Courant number, 𝐶, is less than one. 𝐶 = 𝑢Δ𝑡 Δ𝑥 = ≤ 1, (20.2.66) Since the mesh motion does not occur over any physical time scale, Δt is arbitrary, and uΔt is the transport volume, 𝑓 , between adjacent elements. The transport volume calculation is purely geometrical for ALE formulations and it is not associated with any of the physics of the problem. The algorithms for performing the remap step are taken from the computational fluids dynamics community, and they are referred to as “advection” algorithms after the first order, scalar conservation equation that is frequently used as a model hyperbolic problem. ∂φ ∂t + a(𝑥) ∂φ ∂𝑥 = 0. (20.2.67) A good advection algorithm for the remap step is accurate, stable, conservative and monotonic. Although many of the solution variables, such as the stress and plastic strain, are not governed by conservation equations like momentum and energy, it is still highly desirable that the volume integral of all the solution variables remain unchanged by the remap step. Monotonicity requires that the range of the solution variables does not increase during the remap. This is particularly important with mass and energy, where negative values would lead to physically unrealistic solutions. Much of the research on advection algorithms has focused on developing monotonic algorithms with an accuracy that is at least second order. Not all recent algorithms are monotonic. For example, within the finite element community, the streamline upwind Petrov-Galerkin (SUPG) method developed by Hughes and coworkers [Brooks and Hughes 1982] is not monotonic. Johnson et al., [1984] have demonstrated that the oscillations in the SUPG solution are localized, and its generalization to systems of conservation equations works very well for the Euler equations. Mizukami and Hughes [1985] later developed a monotonic SUPG formulation. The essentially non-oscillatory (ENO) [Harten 1989] finite difference algorithms are also not strictly monotonic, and work well for the Euler equations, but their application to hydrodynamics problems has resulted in negative densities [McGlaun 1990]. Virtually all the higher order methods that are commonly used were originally developed for solving the Euler equations, usually as higher order extensions Simplified Arbitrary Lagrangian-Eulerian LS-DYNA Theory Manual to Godunov’s method. Since the operator split approach is the dominant one in Eulerian hydrocodes, these methods are implemented only to solve the scalar advection equation. The Donor Cell Algorithm. Aside from its first order accuracy, it is everything a good 𝜑 is advection algorithm should be: stable, monotonic, and simple. The value of 𝑓𝑗 dependent on the sign of a at node 𝑗, which defines the upstream direction. 𝑛+1 = φ𝑗+1 φ𝑗+1 2⁄ 2⁄ + Δ𝑡 Δ𝑥 (𝑓𝑗 𝜑 − 𝑓𝑗+1 𝜑 ), 𝜑 = 𝑓𝑗 𝑎𝑗 (φ𝑗−1 2⁄ + φ𝑗+1 2⁄ ) + |𝑎𝑗| (φ𝑗−1 2⁄ − φ𝑗+1 2⁄ ). (20.2.68) (20.2.69) The donor cell algorithm is a first order Godunov method applied to the advection equation. The initial values of 𝜙 to the left and the right of node 𝑗 are φ𝑗−1 2⁄ and φ𝑗+1 2⁄ , and the velocity of the contact discontinuity at node 𝑗 is 𝑎𝑗. The Van Leer MUSCL Algorithm. Van Leer [1977] introduced a family of higher order Godunov methods by improving the estimates of the initial values of left and right states for the Riemann problem at the nodes. The particular advection algorithm that is presented in this section is referred to as the MUSCL (monotone upwind schemes for conservation laws) algorithm for brevity, although MUSCL really refers to the family of algorithms that can be applied to systems of equations. The donor cell algorithm assumes that the distribution of 𝜙 is constant over an element. Van Leer replaces the piecewise constant distribution with a higher order interpolation function, φ𝑗+1 (𝑥) that is subject to an element level conservation 2⁄ constraint. The value of 𝜙 at the element centroid is regarded in this context as the average value of 𝜙 over the element instead of the spatial value at 𝑥𝑗+1 2⁄ . φ𝑗+1 2⁄ 𝑥𝑗+1 = ∫ 𝑥𝑗 φ𝑗+1 2⁄ (𝑥)d𝑥, (20.2.70) min , φ𝑗+1 To determine the range of 𝜙, [φ𝑗+1 2⁄ 2⁄ max ], for imposing the monotonicity constraint, the maximum and minimum values of φ𝑗−1 2⁄ Monotonicity can be imposed in either of two ways. The first is to require that the (𝑥) fall within the range determined by the maximum and minimum values of φ𝑗+1 2⁄ three elements. The second is to restrict the average value of 𝜙 in the transport volumes associated with element 𝑗 + 1/2. While the difference may appear subtle, the actual difference between the two definitions is quite significant even at relatively low Courant numbers. The second definition allows the magnitude of the 𝜙 transported to adjacent , and φ𝑗+3 2⁄ are used. , φ𝑗+1 2⁄ LS-DYNA Theory Manual Simplified Arbitrary Lagrangian-Eulerian elements to be larger than the first definition. As a consequence, the second definition is better able to transport solutions with large discontinuities. The magnitude of 𝜙 an algorithm is able to transport before its monotonicity algorithm restricts 𝜙 is a measure of the algorithm’s “compressiveness.” The first step up from a piecewise constant function is a piecewise linear function, where 𝑥 is now the volume coordinate. The volume coordinate of a point is simply the volume swept along the path between the element centroid and the point. Conservation is guaranteed by expanding the linear function about the element centroid. φ𝑗+1 2⁄ (𝑥) = 𝑆𝑗+1 2⁄ (𝑥 − 𝑥𝑗+1 2⁄ ) + φj+1 2⁄ . (20.2.71) Letting 𝑠𝑗+1 2⁄ be a second order approximation of the slope, the monotonicity limited value of the slope, 𝑠𝑗+1 2⁄ by assuming the maximum permissible values at the element boundaries. , according to the first limiting approach, is determined 𝑆𝑗+1 2⁄ = (sgn(sL) + sgn(sR)) × min (∣sL∣, ∣s𝑗+1 2⁄ ∣ , ∣sR∣), 𝑠L = 𝑠R = − φ𝑗−1 2⁄ φ𝑗+1 2⁄ Δ𝑥𝑗+1 2⁄ − φ𝑗+1 2⁄ φ𝑗+3 2⁄ Δ𝑥𝑗+1 2⁄ , . (20.2.72) (20.2.73) (20.2.74) The second limiter is similar to the first, but it assumes that the maximum permissible values occur at the centroid of the transport volumes. Note that as stated in Equation (17.2.6), this limiter still limits the slope at the element boundary even if the element is the downstream element at that boundary. A more compressive limiter would not limit the slope based on the values of 𝜙 at the downstream boundaries. For example, if 𝑎𝑗 is negative, only 𝑆𝑅 would limit the value of 𝑆𝑛 in Equation (17.2.6). If the element is the downstream element at both boundaries, then the slope in the element has no effect on the solution. Δ𝑥𝑗+1 max(0, 𝑎𝑗Δ𝑡) 𝑠L = 𝑠R = − φ𝑗−1 2⁄ − φ𝑗+1 2⁄ φ𝑗+1 2⁄ 2⁄ − 1 φ𝑗+3 2⁄ 2⁄ + 1 𝑥𝑗+1 min(0, 𝑎𝑗+1Δ𝑡) . . (20.2.75) (20.2.76) Simplified Arbitrary Lagrangian-Eulerian LS-DYNA Theory Manual The flux at node 𝑗 is evaluated using the upstream approximation of 𝜙. φ = 𝑓𝑗 𝑎𝑗 (φ𝑗 − + φ𝑗 +) + |𝑎𝑗| (φ𝑗 − − φ𝑗 +), + = S𝑗+1 φ𝑗 2⁄ (𝑥C − 𝑥𝑗+1 2⁄ ) + φ𝑗+1 2⁄ − = S𝑗−1 φ𝑗 2⁄ (𝑥C − 𝑥𝑗−1 2⁄ ) + φ𝑗−1 2⁄ , , 𝑥C = 𝑥𝑗 𝑛 + 𝑎𝑗Δ𝑡. (20.2.77) (20.2.78) (20.2.79) (20.2.80) The method for obtaining the higher order approximation of the slope is not unique. Perhaps the simplest approach is to fit a parabola through the centroids of the three adjacent elements and evaluate its slope at 𝑥𝑗+1 . When the value of 𝜙 at the 2⁄ element centroids is assumed to be equal to the element average this algorithm defines a projection. (𝜑𝑗+3 2⁄ 𝑠𝑗+1 2⁄ = − φ𝑗+1 2⁄ ) Δ𝑥𝑗 2 + (φ𝑗+1 2⁄ Δ𝑥𝑗Δ𝑥𝑗+1(Δ𝑥𝑗 + Δ𝑥𝑗+1) − φ𝑗−1 2⁄ Δ𝑥𝑗 = 𝑥𝑗+1 2⁄ − 𝑥𝑗−1 2⁄ . ) Δ𝑥𝑗+1 , (20.2.81) (20.2.82) 20.2.2 Advection Methods in Three Dimensions For programs that use a logically regular mesh, one-dimensional advection methods are extended to two and three dimensions by using a sequence of one- dimensional sweeps along the logically orthogonal mesh lines. This strategy is not possible for unstructured meshes because they don’t have uniquely defined sweep directions through the mesh. CAVEAT [Addessio, et al., 1986] uses one-dimensional sweeps in the spatial coordinate system, but their approach is expensive relative to the other algorithms and it does not always maintain spherical symmetry, which is an important consideration in underwater explosion calculations. The advection in LS-DYNA is performed isotropically. The fluxes through each face of element A are calculated simultaneously, but the values of 𝜙 in the transport volumes are calculated using the one-dimensional expressions developed in the previous sections. 𝑛+1 = φA 𝑛+1 VA ⎜⎛VA ⎝ 𝑛 φA 𝑛 + ∑ f𝑗 ⎟⎞. 𝑗=1 ⎠ (20.2.83) LS-DYNA Theory Manual Simplified Arbitrary Lagrangian-Eulerian The disadvantage of isotropic advection is that there is no coupling between an element and the elements that are joined to it only at its corners and edges (i.e., elements that don’t share faces). The lack of coupling introduces a second order error that is significant only when the transport is along the mesh diagonals. The one-dimensional MUSCL scheme, which requires elements on either side of the element whose transport is being calculated, cannot be used on the boundary elements in the direction normal to the boundary. Therefore, in the boundary elements, the donor cell algorithm is used to calculate the transport in the direction that is normal to the boundary, while the MUSCL scheme is used in the two tangential directions. It is implicitly assumed by the transport calculations that the solution variables are defined per unit current volume. In LS-DYNA, some variables, such as the internal energy, are stored in terms of the initial volume of the element. These variables must be rescaled before transport, then the initial volume of the element is advected between the elements, and then the variables are rescaled using the new “initial” volumes. Hyperelastic materials are not currently advected in LS-DYNA because they require the deformation gradient, which is calculated from the initial geometry of the mesh. If the deformation gradient is integrated by using the midpoint rule, and it is advected with the other solution variables, then hyperelastic materials can be advected without any difficulties. F𝑛+1 = (I − Δ𝑡 2L𝑛+1 2⁄ )−1 (I + Δ𝑡 2L𝑛+1 2⁄ ) F𝑛. (20.2.84) Advection of the Nodal Velocities. Except for the Godunov schemes, the velocity is centered at the nodes or the edges while the remaining variables are centered in the elements. Momentum is advected instead of the velocity in most codes to guarantee that momentum is conserved. The element-centered advection algorithms must be modified to advect the node-centered momentum. Similar difficulties are encountered when node-centered algorithms, such as the SUPG method [Brooks and Hughes 1982], are applied to element-centered quantities [Liu, Chang, and Belytschko, to be published]. There are two approaches: 1) construct a new mesh such that the nodes become the element centroids of the new mesh and apply the element-centered advection algorithms, and 2) construct an auxiliary set of element-centered variables from the momentum, advect them, and then reconstruct the new velocities from the auxiliary variables. Both approaches can be made to work well, but their efficiency is heavily dependent on the architecture of the codes. The algorithms are presented in detail for one dimension first for clarity. Their extensions to three dimensions, which are presented later, are straightforward even if the equations do become lengthy. A detailed discussion of the algorithms in two dimensions is presented in Reference [Benson 1992]. Simplified Arbitrary Lagrangian-Eulerian LS-DYNA Theory Manual Notation. Finite difference notation is used in this section so that the relative locations of the nodes and fluxes are clear. The algorithms are readily applied, however, to unstructured meshes. To avoid limiting the discussion to a particular element-centered advection algorithm, the transport volume through node 𝑖 is 𝑓 , the transported mass is 𝑓 ̃ 𝑖, and the flux of 𝜙 is 𝜙𝑖𝑓𝑖. Most of the element-centered flux-limited advection algorithms calculate the flux of 𝜙 directly, but the mean value of 𝜙 in the transport volumes is calculated by dividing the 𝜙i𝑓i, by the transport volume. A superscript “-” or “+” denotes the value of a variable before or after the advection. Using this notation, the advection of 𝜙 in one dimension is represented by Equation (17.2.12), where the volume is V. + φ𝑗+1 2⁄ = − V𝑗+1 (φ𝑗+1 2⁄ 2⁄ − + φ𝑖𝑓𝑖 − φ𝑖+1𝑓𝑖+1) , V+ + V𝑗+1 2⁄ − = V𝑗+1 2⁄ + 𝑓𝑖 − 𝑓𝑖+1. (20.2.85) (20.2.86) The Staggered Mesh Algorithm. YAQUI [Amsden and Hirt 1973] was the first code to construct a new mesh that is staggered with respect to original mesh for momentum advection. The new mesh is defined so that the original nodes become the centroids of the new elements. The element-centered advection algorithms are applied to the new mesh to advect the momentum. In theory, the momentum can be advected with the transport volumes or the velocity can be advected with the mass. (M𝑗 −v𝑗 − + v𝑗−1 + = v𝑗 2⁄ − v𝑗+1 2⁄ 𝑓 ̃ 𝑗+1 2⁄ ) , (M𝑗 −v𝑗 − + {ρv}𝑗−1 + = v𝑗 2⁄ − {ρv}𝑗+1 2⁄ 𝑓𝑗−1 2⁄ ) , 2⁄ 𝑓 ̃ 𝑗−1 + M𝑗 2⁄ 𝑓𝑗−1 + M𝑗 M𝑗 + = M𝑗 − + 𝑓 ̃ 𝑗−1 2⁄ − 𝑓 ̃ 𝑗+1 2⁄ . (20.2.87) (20.2.88) (20.2.89) A consistency condition, first defined by DeBar [1974], imposes a constraint on the formulation of the staggered mesh algorithm: if a body has a uniform velocity and a spatially varying density before the advection, then the velocity should be uniform and unchanged after the advection. The new mass of a node can be expressed in terms of the quantities used to advect the element-centered mass. + = M𝑗 + (M𝑗−1 2⁄ + + M𝑗+1 2⁄ ), + = M𝑗 − (M𝑗−1 2⁄ − + 𝜌𝑗−1𝑓𝑗−1 − 𝜌𝑗𝑓𝑗 + M𝑗+1 2⁄ + 𝜌𝑗𝑓𝑗 − 𝜌𝑗+1𝑓𝑗+1), (20.2.90) (20.2.91) LS-DYNA Theory Manual Simplified Arbitrary Lagrangian-Eulerian M𝑗 + = M𝑗 − + [(𝜌𝑗−1𝑓𝑗−1 − 𝜌𝑗𝑓𝑗) + (𝜌𝑗𝑓𝑗 − 𝜌𝑗+1𝑓𝑗+1)]. (20.2.92) The staggered mass fluxes and transport volumes are defined by equating Equation (20.2.90) and Equation (17.2.15). 𝜌𝑗+1 2⁄ 𝑓𝑗+1 2⁄ = 𝑓 ̃ 𝑗+1 2⁄ = (𝜌𝑗𝑓𝑗 + 𝜌𝑗+1𝑓𝑗+1). (20.2.93) 2⁄ is generally a nonlinear function of the volume 𝑓𝑗+1 2⁄ , hence The density 𝜌𝑗+1 calculating 𝑓𝑗+1 2⁄ from Equation (20.2.93) requires the solution of a nonlinear equation for each transport volume. In contrast, the mass flux is explicitly defined by Equation (20.2.93). Most codes, including KRAKEN [Debar 1974], CSQ [Thompson 1975], CTH [McGlaun 1989], and DYNA2D [Hallquist 1980], use mass fluxes with the staggered mesh algorithm because of their simplicity. The dispersion characteristics of this algorithm are identical to the underlying element-centered algorithm by construction. This is not true, however, for some of the element-centered momentum advection algorithms. There are some difficulties in implementing the staggered mesh method in multi-dimensions. First, the number of edges defining a staggered element equals the number of elements surrounding the corresponding node. On an unstructured mesh, the arbitrary connectivity results in an arbitrary number of edges for each staggered element. Most of the higher order accurate advection algorithms assume a logically regular mesh of quadrilateral elements, making it difficult to use them with the staggered mesh. Vectorization also becomes difficult because of the random number of edges that each staggered element might have. In the ALE calculations of DYNA2D, only the nodes that have a locally logically regular mesh surrounding them can be moved in order to avoid these difficulties [Benson 1992]. These difficulties do not occur in finite difference codes which process logically regular blocks of zones. Another criticism is the staggered mesh algorithm tends to smear out shocks because not all the advected variables are element-centered [Margolin 1989]. This is the primary reason, according to Margolin [1989], that the element-centered algorithm was adopted in SALE [Amdsden, Ruppel, and Hirt 1980]. The SALE Algorithm. SALE advects an element-centered momentum and redistributes its changes to the nodes [Amdsden, Ruppel, and Hirt 1980]. The mean element velocity, 𝐯̅̅̅̅𝑗+1 2⁄ , and nodal momentum 2⁄ , specific momentum, 𝐩𝑗+1 are defined by Equation (17.2.17). 2⁄ , element momentum, 𝐏𝑗+1 𝐯̅̅̅̅𝑗+1 2⁄ = (𝐯𝑗 + 𝐯𝑗+1), 𝐩𝑗+1 2⁄ = ρ𝑗+1 2⁄ 𝐯̅̅̅̅𝑗+1 2⁄ , 𝐏j+1 2⁄ = M𝑗+1 2⁄ 𝐯̅̅̅̅𝑗+1 2⁄ . (20.2.94) (20.2.95) (20.2.96) Simplified Arbitrary Lagrangian-Eulerian LS-DYNA Theory Manual 2⁄ , the change in the velocity at a Denoting the change in the element momentum Δ𝐏𝑗+1 node is calculated by distributing half the momentum change from the two adjacent elements. Δ𝐏𝑗−1 2⁄ = p𝑗−1𝑓𝑗−1 − p𝑗𝑓𝑗, + = P𝑗 P𝑗 − + (Δ𝐏𝑗−1 2⁄ + Δ𝐏𝑗+1 2⁄ ), + = 𝐯𝑗 + 𝐏𝑗 +. M𝑗 (20.2.97) (20.2.98) (20.2.99) This algorithm can also be implemented by advecting the mean velocity, 𝐯̅̅̅̅𝑗+1 2⁄ with the transported mass, and the transported momentum 𝐩𝑗𝑓𝑗 is changed to 𝐯̅̅̅̅𝑗𝑓 ̃ 𝑗. The consistency condition is satisfied regardless of whether masses or volumes are used. Note that the velocity is not updated from the updated values of the adjacent element momenta. The reason for this is the original velocities are not recovered if 𝑓𝑖 = 0, which indicates that there is an inversion error associated with the algorithm. The HIS (Half Index Shift) Algorithm. Benson [1992] developed this algorithm based on his analysis of other element-centered advection algorithms. It is designed to overcome the dispersion errors of the SALE algorithm and to preserve the monotonicity of the velocity field. The SALE algorithm is a special case of a general class of algorithms. To sketch the idea behind the HIS algorithm, the discussion is restricted to the scalar advection equation. Two variables, Ψ1,𝑗+1 2⁄ are defined in terms of a linear transformation of 𝜙𝑗 and 𝜙𝑗+1. The linear transformation may be a function of the element 𝑗 + 1/2. 2⁄ and Ψ2,𝑗+1 − {⎧Ψ1,𝑗+1 2⁄ − ⎩{⎨ Ψ2,𝑗+1 2⁄ }⎫ ⎭}⎬ = [a b c d ] { − φ𝑗 − }. φ𝑗+1 This relation is readily inverted. { + φ𝑗 + } = φ𝑗+1 ad − bc −b [d −c a ] + {⎧Ψ1,𝑗+1 2⁄ ⎩{⎨ + Ψ2,𝑗+1 2⁄ }⎫ ⎭}⎬ . (20.2.100) (20.2.101) A function is monotonic over an interval if its derivative does not change sign. The sum of two monotonic functions is monotonic, but their difference is not necessarily are monotonic over the same monotonic. As a consequence, Ψ1,𝑗+1 2⁄ − if all the coefficients in the linear transformation have the same sign. On intervals as φ𝑗 are the other hand, φ𝑗 + is not necessarily monotonic even if Ψ1,𝑗+1 2⁄ and Ψ2,𝑗+1 2⁄ and Ψ2,𝑗+1 2⁄ + + − − LS-DYNA Theory Manual Simplified Arbitrary Lagrangian-Eulerian monotonic because of the appearance of the negative signs in the inverse matrix. Monotonicity can be maintained by transforming in both directions provided that the transformation matrix is diagonal. Symmetry in the overall algorithm is obtained by using a weighted average of the values of 𝜙𝑗 calculated in elements 𝑗 + 1/2 and 𝑗 − 1/2. A monotonic element-centered momentum advection algorithm is obtained by choosing the identity matrix for the transformation and by using mass weighting for the inverse relationship. {⎧Ψ1,𝑗+1 }⎫ 2⁄ 2⁄ ⎭}⎬ ⎩{⎨ Ψ2,𝑗+1 To conserve momentum, Ψ is advected with the transport masses. − v𝑗 − } v𝑗+1 = [1 ] { (M − Ψ 𝑗+1 − 𝑚,𝑗+1 + Ψ𝑚,𝑗+1/2 = + Ψ𝑚,𝑗 − 𝑓 ̃ − 𝑗 − Ψ𝑚,𝑗+1 + 𝑗+1 𝑓 ̃ 𝑗+1) , (20.2.102) (20.2.103) v𝑗 = 2M𝑗 (M𝑗+1/2Ψ1,𝑗+1/2 + M𝑗−1/2Ψ2,𝑗−1/2). (20.2.104) Dispersion Errors. A von Neumann analysis [Trefethen 1982] characterizes the dispersion errors of linear advection algorithms. Since the momentum advection the algorithm modifies momentum advection algorithm does not necessarily have the same dispersion characteristics as the underlying algorithm. The von Neumann analysis provides a tool to explore the changes in the dispersion characteristics without considering a particular underlying advection algorithm. the underlying element-centered advection algorithm, The model problem is the linear advection equation with a constant value of c. A class of solutions can be expressed as complex exponentials, where i is √−1 , ω is the frequency, and χ is the wave number. ∂φ ∂𝑡 + c ∂φ ∂𝑥 = 0, φ(𝑥, 𝑡) = 𝑒𝑖(ω𝑡−χ𝑥). (20.2.105) (20.2.106) For Equation (17.2.24), the dispersion equation is 𝜔 = 𝑐𝜒, but for discrete approximations of the equation and for general hyperbolic equations, the relation is 𝜔 = 𝜔𝜒. The phase velocity, cp, and the group speed, cg, are defined by Equation (17.2.25). cp = , (20.2.107) Simplified Arbitrary Lagrangian-Eulerian LS-DYNA Theory Manual cg = ∂ω . ∂χ (20.2.108) The mesh spacing is assumed to have a constant value 𝐽, and the time step, ℎ, is also constant. The + and - states in the previous discussions correspond to times n and n + 1 in the dispersion analysis. An explicit linear advection method that has the form given by Equation (1.2.109) results in a complex dispersion equation, Equation (17.2.27), where Π is a complex polynomial. 𝑛+1 = 𝜑𝑗 𝜑𝑗 𝑛 + F(c, ℎ, 𝐽, . . . , 𝜑𝑗−1 𝑛 , 𝜑𝑗, 𝑛𝜑𝑗+1 𝑛 , . . . ), 𝑒𝑖ωℎ = 1 + P(𝑒𝑖χ𝐽), Π(𝑒𝑖χ𝐽) = ∑ 𝛽𝑗𝑒𝑖χ𝑗𝐽 . (20.2.109) (20.2.110) (20.2.111) The dispersion equation has the general form given in Equation (1.2.112), where Πr and Πi denote the real and imaginary parts of Π, respectively. Π𝑖 1 + Πr Recognizing that the relations in the above equations are periodic in 𝜔ℎ and χ𝐽, the normalized frequency and wave number are defined to simplify the notation. ωℎ = tan−1 ( (20.2.112) ). 𝜔̅̅̅̅ = ωℎ, χ̅̅̅̅ = χ𝐽. (20.2.113) The von Neumann analysis of the SALE algorithm proceeds by first calculating the increment in the cell momentum. p𝑗+1/2 = (v𝑗 𝑛 + v𝑗+1 𝑛 ), p𝑗+1/2 = 𝑛, (1 + 𝑒−𝑖χ̅̅̅̅̅)v𝑗 Δp𝑗+1/2 𝑛+1 = P𝑗+1 2⁄ 𝑛+1 − P𝑗+1 2⁄ , Δp𝑗+1/2 𝑛+1 = 𝑛. (1 + e−𝑖χ̅̅̅̅̅)Πv𝑗 The velocity is updated from the changes in the cell momentum. 𝑛+1 = v𝑗 v𝑗 𝑛 + (Δp𝑗+1/2 𝑛+1 + Δp𝑗−1/2 𝑛+1 ), 𝑛+1 = v𝑗 𝑛, (1 + 𝑒𝑖χ̅̅̅̅̅)(1 + 𝑒−𝑖χ̅̅̅̅̅)Πv𝑗 (20.2.114) (20.2.115) (20.2.116) (20.2.117) (20.2.118) (20.2.119) LS-DYNA Theory Manual Simplified Arbitrary Lagrangian-Eulerian 𝑛+1 = v𝑗 𝑛. (1 + cos(χ̅̅̅̅))Πv𝑗 (20.2.120) The dispersion relation for the SALE advection algorithm is given by Equation (1.2.121). 𝜔̅̅̅̅ = tan−1 ⎜⎜⎜⎛ ⎝ 1 + 1 (1 + cos(χ̅̅̅̅))Π𝑖 ⎟⎟⎟⎞ (1 + cos(χ̅̅̅̅))Πr⎠ . (20.2.121) By comparing Equation (20.2.112) and Equation (20.2.121), the effect of the SALE momentum advection algorithm on the dispersion is to introduce a factor λ, equal to 2 (1 + cos(χ̅̅̅̅))Π, into the spatial part of the advection stencil. For small values of χ̅̅̅̅, λ is close to one, and the dispersion characteristics are not changed, but when χ̅̅̅̅ is π, the phase and group velocity go to zero and the amplification factor is one independent of the underlying advection algorithm. Not only is the wave not transported, it is not damped out. The same effect is found in two dimensions, where λ, has the form 4 (1 + cos(χ̅̅̅̅) + cos(χ̅̅̅̅̅̅̅̅) + cos(χ̅̅̅̅)cos(χ̅̅̅̅̅̅̅̅)). In contrast, none of the other algorithms alter the dispersion characteristics of the underlying algorithm. Benson has demonstrated for the element-centered algorithms that the SALE inversion error and the dispersion problem are linked. Algorithms that fall into the same general class as the SALE and HIS algorithms will, therefore, not have dispersion problems [Benson 1992]. Three-Dimensional Momentum Advection Algorithms. The momentum advection algorithms discussed in the previous sections are extended to three dimensions in a straightforward manner. The staggered mesh algorithm requires the construction of a staggered mesh and the appropriate transport masses. Based on the consistency arguments, the appropriate transport masses are given by Equation (1.2.122). 𝑓 ̃ 𝑗+1/2,𝑘,𝑙 = 𝑙+1 2⁄ 𝑘+1 2⁄ 𝑗+1 ∑ ∑ ∑ 𝑓𝐽,𝐾,𝐿 𝐽=𝑗 𝐾=𝑘−1 𝐿=𝑙−1 2⁄ 2⁄ . (20.2.122) The SALE advection algorithm calculates the average momentum of the element from the four velocities at the nodes and distributes 1⁄8 of the change in momentum to each node. p𝑗+1 2⁄ ,𝑘+1 2⁄ ,𝑙+1 2⁄ = 𝑗+1 𝑘+1 𝑙+1 𝜌𝑗+1 2⁄ ,𝑘+1 2⁄ ,𝑙+1 2⁄ ∑ ∑ ∑ v𝐽𝐾𝐿 𝐽=𝑗 𝐾=𝑘 𝐿=𝑙 , (20.2.123) Simplified Arbitrary Lagrangian-Eulerian LS-DYNA Theory Manual p𝑗+1 2⁄ ,𝑘+1 2⁄ ,𝑙+1 2⁄ = 𝑗+1 𝑘+1 𝑙+1 𝑀𝑗+1 2⁄ ,𝑘+1 2⁄ ,𝑙+1 2⁄ ∑ ∑ ∑ v𝐽𝐾𝐿 𝐽=𝑗 𝐾=𝑘 𝐿=𝑙 , (20.2.124) + = v𝑗,𝑘,𝑙 + 𝑀𝑗,𝑘,𝑙 ⎜⎜⎜⎛ ⎝ 𝑀𝑗,𝑘,𝑙 − 𝑣𝑗,𝑘,𝑙 − + 2⁄ 𝑘+1 𝑗+1 ∑ ∑ ∑ 𝛥𝑃𝐽,𝐾,𝐿 𝑙+1 2⁄ 2⁄ 𝐽=𝑗−1 2⁄ 𝐾=𝑘−1 2⁄ 𝐿=𝑙−1 2⁄ . ⎟⎟⎟⎞ ⎠ (20.2.125) The HIS algorithm is also readily extended to three dimensions. The variable definitions are given in Equation (1.2.126) and Equation (1.2.127), where the subscript A refers to the local numbering of the nodes in the element. In an unstructured mesh, the relative orientation of the nodal numbering within the elements may change. The subscript A is always with reference to the numbering in element 𝑗, 𝑘, 𝑙. The subscript à is the local node number in an adjacent element that refers to the same global node number as A. ΨA,𝑗+1 2⁄ ,𝑘+1 2⁄ ,𝑙+1 2⁄ = vA,𝑗+1 2⁄ ,𝑘+1 2⁄ ,𝑙+1 2⁄ , + = v𝑗,𝑘,𝑙 2⁄ 𝑗+1 𝑘+1 𝑙+1 + ∑ ∑ ∑ MJ,K,LΨÃ,J,K,L M𝑗,𝑘,𝑙 𝐿=𝑙−1 𝐾=𝑘−1 𝐽=𝑗−1 2⁄ 2⁄ + 2⁄ 2⁄ 2⁄ (20.2.126) . (20.2.127) 20.3 The Manual Rezone The central limitation to the simplified ALE formulation is that the topology of the mesh is fixed. For a problem involving large deformations, a mesh that works well at early times may not work at late times regardless of how the mesh is distributed over the material domain. To circumvent this difficulty, a manual rezoning capability has been implemented in LS-DYNA. The general procedure is to 1) interrupt the calculation when the mesh is no longer acceptable, 2) generate a new mesh with INGRID by using the current material boundaries from LS-DYNA (the topologies of the new and old mesh are unrelated), 3) remap the solution from the old mesh to the new mesh, and 4) restart the calculation. This chapter will concentrate on the remapping algorithm since the mesh generation capability is documented in the INGRID manual [Stillman and Hallquist 1992]. The remapping algorithm first constructs an interpolation function on the original mesh by using a least squares procedure, and then interpolates for the solution values on the new mesh. The one point quadrature used in LS-DYNA implies a piecewise constant distribution of the solution variables within the elements. A piecewise constant LS-DYNA Theory Manual Simplified Arbitrary Lagrangian-Eulerian distribution is not acceptable for a rezoner since it implies that for even moderately large changes in the locations of the nodes (say, displacements on the order of fifty percent of the elements characteristic lengths) that there will be no changes in the values of the element-centered solution variables. A least squares algorithm is used to generate values for the solution variables at the nodes from the element-centered values. The values of the solution variables can then be interpolated from the nodal values, 𝜙A, using the standard trilinear shape functions anywhere within the mesh. 𝜙(𝜉 , 𝜂, 𝜁 ) = 𝜙𝐴NA(𝜉 , 𝜂, 𝜁 ). (20.3.128) The objective function for minimization, 𝐽, is defined material by material, and each material is remapped independently. 𝐽 = ∫(φA NA − φ)2dV. (20.3.129) The objective function is minimized by setting the derivatives of 𝐽 with respect to 𝜙𝐴 equal to zero. ∂𝐽 ∂φA = ∫(φB NB − φ)NAdV = 0. (20.3.130) The least square values of 𝜙A are calculated by solving the system of linear equations, Equation (17.3.4). MABφB = ∫ NA φdV, MAB = ∫ NA NBdV. (20.3.131) (20.3.132) The “mass matrix”, MAB, is lumped to give a diagonal matrix. This eliminates the spurious oscillations that occur in a least squares fit around the discontinuities in the solution (e.g., shock waves) and facilitates an explicit solution for 𝜙A. The integral on the right hand side of Equation (20.3.131) is evaluated using one point integration. By introducing these simplifications, Equation (17.3.4) is reduced to Equation (1.3.133), where the summation over a is restricted to the elements containing node A. φA = ∑ φαVα ∑ Vαα . (20.3.133) The value of 𝜙α is the mean value of 𝜙 in element a. From this definition, the value of 𝜙α is calculated using Equation (1.3.134). φα = Vα ∫ φA Vα NAdV. (20.3.134) Simplified Arbitrary Lagrangian-Eulerian LS-DYNA Theory Manual The integrand in Equation (20.3.134) is defined on the old mesh, so that Equation (20.3.134) is actually performed on the region of the old mesh that overlaps element α in the new mesh, where the superscript “*” refers to elements on the old mesh. φα = Vα ∑ ∗ ∫ φA NAdV∗. ∗ Vα∩Vβ (20.3.135) One point integration is currently used to evaluate Equation (20.3.135), although it would be a trivial matter to add higher order integration. By introducing this simplification, Equation (20.3.135) reduces to interpolating the value of 𝜙𝛼 from the least squares fit on the old mesh. 𝜙a = 𝜙ANA(𝜉 ∗, 𝜂∗, 𝜁 ∗). (20.3.136) The isoparametric coordinates in the old mesh that correspond to the spatial location of the new element centroid must be calculated for Equation (20.3.136). The algorithm that is described here is from Shapiro [1990], who references [Thompson and Maffeo 1985, Maffeo 1984, Maffeo 1985] as the motivations for his current strategy, and we follow his notation. The algorithm uses a “coarse filter” and a “fine filter” to make the search for the correct element in the old mesh efficient. The coarse filter calculates the minimum and maximum coordinates of each element in the old mesh. If the new element centroid, (𝑥𝑠, 𝑦𝑠, 𝑧𝑠), lies outside of the box defined by the maximum and minimum values of an old element, then the old element does not contain the new element centroid. Several elements may pass the coarse filter but only one of them contains the new centroid. The fine filter is used to determine if an element actually contains the new centroid. The fine filter algorithm will be explained in detail for the two- dimensional case since it easier to visualize than the three-dimensional case, but the final equations will be given for the three-dimensional case. The two edges adjacent to each node in Figure 20.2 (taken from [Shapiro 1990]) define four skew coordinate systems. If the coordinates for the new centroid are positive for each coordinate system, then the new centroid is located within the old element. Because of the overlap of the four positive quarter spaces defined by the skew coordinate systems, only two coordinate systems actually have to be checked. Using the first and third coordinate systems, the coordinates, α𝑖, are the solution of Equation (17.3.9). 𝑉𝑠 = 𝑉1 + 𝑎1𝑉12 + 𝑎2𝑉14, 𝑉𝑠 = 𝑉3 + 𝑎3𝑉32 + 𝑎4𝑉34. (20.3.137) (20.3.138) LS-DYNA Theory Manual Simplified Arbitrary Lagrangian-Eulerian 3v32 (xs, ys) 1v12 v1 vs 4v34 2v14 Figure 20.2. Skew Coordinate System Two sets of linear equations are generated for the α𝑖 by expanding the vector equations. [ 𝑥2 − 𝑥1 𝑦2 − 𝑦1 𝑥4 − 𝑥1 𝑦4 − 𝑦1 ] { [ 𝑥2 − 𝑥3 𝑦2 − 𝑦3 𝑥4 − 𝑥3 𝑦4 − 𝑦3 ] { 𝛼1 𝛼2 𝛼3 𝛼4 } = { 𝑥𝑠 − 𝑥1 𝑦𝑠 − 𝑦1 } = { 𝑥𝑠 − 𝑥3 𝑦𝑠 − 𝑦3 }, }. (20.3.139) (20.3.140) The generalization of Equation (17.3.9) to three dimensions is given by Equation (17.3.11), and it requires the solution of four sets of three equations. The numbering convention for the nodes in Equation (17.3.11) follows the standard numbering scheme used in LS-DYNA for eight node solid elements. 𝑉s = 𝑉1 + 𝑎1𝑉12 + 𝑎2𝑉14 + 𝑎3𝑉15, 𝑉s = 𝑉3 + 𝑎4𝑉37 + 𝑎5𝑉34 + 𝑎6𝑉32, 𝑉s = 𝑉6 + 𝑎7𝑉62 + 𝑎8𝑉65 + 𝑎9𝑉67, 𝑉s = 𝑉8 + 𝑎10𝑉85 + 𝑎11𝑉84 + 𝑎12𝑉87. (20.3.141) (20.3.142) (20.3.143) (20.3.144) The fine filter sometimes fails to locate the correct element when the mesh is distorted. When this occurs, the element that is closest to the new centroid is located by finding the element for which the sum of the distances between the new centroid and the nodes of the element is a minimum. Simplified Arbitrary Lagrangian-Eulerian LS-DYNA Theory Manual Once the correct element is found, the isoparametric coordinates are calculated using the Newton-Raphson method, which usually converges in three or four iterations. 𝑦A ⎡𝑥A ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎣ 𝑧A ∂𝑁A ∂𝜉 ∂𝑁A ∂𝜉 ∂𝑁A ∂𝜉 𝑥A 𝑦A 𝑧A ∂𝑁A ∂𝜂 ∂𝑁A ∂𝜂 ∂𝑁A ∂𝜂 𝑥A 𝑦A 𝑧A ∂𝑁A ⎤ ∂𝜁 ⎥ ⎥ ∂𝑁A ⎥ ⎥ ∂𝜁 ⎥ ⎥ ∂𝑁A ⎥ ∂𝜁 ⎦ {⎧Δ𝜉 }⎫ Δ𝜂 Δ𝜁 ⎭}⎬ ⎩{⎨ = {⎧𝑥s − 𝑥A𝑁A }⎫ 𝑦s − 𝑦A𝑁A , 𝑧s − 𝑧A𝑁A ⎭}⎬ ⎩{⎨ 𝜉 𝑖+1 = 𝜉 𝑖 + 𝛥𝜉 , 𝜂𝑖+1 = 𝜂𝑖 + 𝛥𝜂, 𝜁 𝑖+1 = 𝜁 𝑖 + 𝛥𝜁 . (20.3.145) (20.3.146) LS-DYNA Theory Manual Stress Update Overview 21 Stress Update Overview 21.1 Jaumann Stress Rate Stresses for material which exhibit elastic-plastic and soil-like behavior (hypoelastic) are integrated incrementally in time: 𝜎𝑖𝑗(𝑡 + 𝑑𝑡) = 𝜎𝑖𝑗(𝑡) + 𝜎̇𝑖𝑗𝑑𝑡, (21.1) Here, and in equations which follow, we neglect the contribution of the bulk viscosity to the stress tensor. In Equation (21.1), the dot denotes the material time derivative given by in which is the spin tensor and 𝜎̇𝑖𝑗 = 𝜎𝑖𝑗 ∇ + 𝜎𝑖𝑘𝜔𝑘𝑗 + 𝜎𝑗𝑘𝜔𝑘𝑖, 𝜔𝑖𝑗 = ( ∂𝑣𝑖 ∂𝑥𝑗 − ∂𝑣𝑗 ∂𝑥𝑖 ), ∇ = 𝐶𝑖𝑗𝑘𝑙𝜀̇𝑘𝑙, 𝜎𝑖𝑗 (21.2) (21.3) (21.4) is the Jaumann (co-rotational) stress rate. In Equation (21.4), 𝐶𝑖𝑗𝑘𝑙 is the stress dependent constitutive matrix, 𝑣𝑖, is the velocity vector, and 𝜀̇𝑖𝑗 is the strain rate tensor: 𝜀̇𝑖𝑗 = ( ∂𝑣𝑖 ∂𝑥𝑗 + ∂𝑣𝑗 ∂𝑥𝑖 ). (21.5) In the implementation of Equation (21.1) we first perform the stress rotation, Equation (21.2), and then call a constitutive subroutine to add the incremental stress components 𝜎𝑖𝑗 𝛻 . This may be written as 𝑛+1 = 𝜎𝑖𝑗 𝜎𝑖𝑗 𝑛 + 𝑟𝑖𝑗 𝑛 + 𝜎𝑖𝑗 𝛻𝑛+1 2⁄ Δ𝑡𝑛+1 2⁄ , (21.6) Stress Update Overview LS-DYNA Theory Manual where 𝛻𝑛+1 2⁄ 𝜎𝑖𝑗 𝑛+1 2⁄ Δ𝜀𝑖𝑗 𝑛+1 2⁄ Δ𝑡𝑛+1 2⁄ = 𝐶𝑖𝑗𝑘𝑙Δ𝜀𝑘𝑙 𝑛+1 Δ𝑡𝑛+1 2⁄ 2⁄ , = 𝜀̇𝑖𝑗 , and 𝑟𝑖𝑗 𝑛 gives the rotation of the stress at time 𝑡𝑛 to the configuration at 𝑡𝑛 + 1 𝑛 = (𝜎𝑖𝑝 𝑟𝑖𝑗 𝑛 𝜔𝑝𝑗 𝑛+1 2⁄ + 𝜎𝑗𝑝 𝑛 𝜔𝑝𝑖 𝑛+1 2⁄ ) Δ𝑡𝑛+1 2⁄ . (21.7) (21.8) In the implicit NIKE2D/3D [Hallquist 1981b] codes, which are used for low frequency structural response, we do a half-step rotation, apply the constitutive law, and complete the second half-step rotation on the modified stress. This approach has also been adopted for some element formulations in LS-DYNA when the invariant stress update is active. An exact or second order accurate rotation is performed rather than the approximate one represented by Equation (21.3), which is valid only for small incremental rotations. A typical implicit time step is usually 100 to 1000 or more times larger than the explicit time step; consequently, the direct use of Equation (21.7) could lead to very significant errors. 21.2 Jaumann Stress Rate Used With Equations of State If pressure is defined by an equation of state as a function of relative volume, 𝑉, and energy, 𝐸, or temperature, 𝑇, we update the deviatoric stress components 𝑝 = 𝑝(𝑉, 𝐸) = 𝑝(𝑉, 𝑇), 𝑛+1 2⁄ where 𝜀̇′𝑖𝑗 𝑛+1 = 𝜎𝑖𝑗 𝑠𝑖𝑗 𝑛 + 𝑟𝑖𝑗 𝑛 + 𝑝𝑛𝛿𝑖𝑗 + 𝐶𝑖𝑗𝑘𝑙𝜀̇′𝑘𝑙 𝑛+1 2⁄ is the deviatoric strain rate tensor: 𝑛+1 2⁄ 𝜀̇′𝑖𝑗 = 𝜀̇𝑖𝑗 − 𝜀̇𝑘𝑘𝛿. 𝛥𝑡𝑛+1 2⁄ , (21.9) (21.10) (21.11) Before the equation of state, Equation (21.9), is evaluated, we compute the bulk viscosity, 𝑞, and update the total internal energy 𝑒 of the element being processed to a trial value 𝑒∗: 𝑒∗𝑛+1 = 𝑒𝑛 − Δ𝑣 (𝑝𝑛 + 𝑞𝑛−1 2⁄ + 𝑞𝑛+1 2⁄ ) + 𝑣𝑛+1 𝑛+1 2⁄ 2⁄ 𝑠𝑖𝑗 𝑛+1 2⁄ Δ𝜀𝑖𝑗 , (21.12) where 𝑣 is the element volume and LS-DYNA Theory Manual Stress Update Overview Δ𝑣 = 𝑣𝑛+1 − 𝑣𝑛, 𝑣𝑛+1 The time-centering of the viscosity is explained by Noh [1976]. (𝑣𝑛 + 𝑣𝑛+1), 2⁄ = 2 = 𝑛+1 𝑠𝑖𝑗 (𝑠𝑖𝑗 𝑛 + 𝑠𝑖𝑗 𝑛+1). (21.13) Assume we have an equation of state that is linear in internal energy of the form where 𝑝𝑛+1 = 𝐴𝑛+1 + 𝐵𝑛+1𝐸𝑛+1, 𝐸𝑛+1 = 𝑒𝑛+1 𝑣0 , and 𝜐0 is the initial volume of the element. Noting that 𝑒𝑛+1 = 𝑒∗𝑛+1 − Δ𝑣𝑝𝑛+1, pressure can be evaluated exactly by solving the implicit form 𝑝𝑛+1 = (𝐴𝑛+1 + 𝐵𝑛+1𝐸∗𝑛+1) , (1 + 1 𝐵𝑛+1 Δ𝑣 𝑣0 ) (21.14) (21.15) (21.16) (21.17) and the internal energy can be updated in Equation (21.16). If the equation of state is not linear in internal energy, a one-step iteration is used to approximate the pressure 𝑝∗𝑛+1 = 𝑝(𝑉𝑛+1, 𝐸∗𝑛+1). (21.18) Internal energy is updated to 𝑛 + 1 using 𝑝∗𝑛+1 in Equation (21.16) and the final pressure is then computed: 𝑝𝑛+1 = 𝑝(𝑉𝑛+1, 𝐸𝑛+1). (21.19) This is also the iteration procedure used in KOVEC [Woodruff 1973]. All the equations of state in LS-DYNA are linear in energy except the ratio of polynomials. 21.3 Green-Naghdi Stress Rate The Green-Naghdi rate is defined as 𝛻 = 𝜎̇𝑖𝑗 + 𝜎𝑖𝑘𝛺𝑘𝑗 + 𝜎𝑗𝑘𝛺𝑘𝑖 = 𝑅𝑖𝑘𝑅𝑗𝑙𝜏̇ 𝜎𝑖𝑗 , 𝑘𝑙 where 𝛺𝑖𝑗 is defined as 𝛺𝑖𝑗 = 𝑅̇ 𝑖𝑘𝑅𝑖𝑘, and 𝐑 is found by application of the polar decomposition theorem 𝐹𝑖𝑗 = 𝑅𝑖𝑘𝑈𝑘𝑗 = 𝑉𝑖𝑘𝑅𝑘𝑗, (21.20) (21.21) (21.22) Stress Update Overview LS-DYNA Theory Manual 𝐹𝑖𝑗 is the deformation gradient matrix and 𝑈𝑖𝑗 and 𝑉𝑖𝑗 are the positive definite right and left stretch tensors: 𝐹𝑖𝑗 = 𝜕𝑥𝑖 𝜕𝑋𝑗 . (21.23) Stresses are updated for all materials by adding to the rotated Cauchy stress at time n. the stress increment obtained by an evaluation of the constitutive equations, 𝑛 = 𝑅𝑘𝑖 𝜏𝑖𝑗 𝑛 𝑅𝑙𝑗 𝑛, 𝑛𝜎𝑘𝑙 𝑛+1 2⁄ Δ𝜏𝑖𝑗 where = 𝐶𝑖𝑗𝑘𝑙 Δ𝑑𝑘𝑙 𝑛+1 2⁄ , 𝑛+1 2⁄ Δ𝑑𝑖𝑗 𝑛+1 2⁄ = 𝑅𝑘𝑖 𝑛+1 2⁄ 𝑅𝑙𝑗 𝑛+1 2⁄ Δ𝜀𝑘𝑙 𝐶𝑖𝑗𝑘𝑙 Δ𝜀𝑘𝑙 = = constitutive matrix increment in strain and to obtain the rotated Cauchy stress at 𝑡𝑛+1, i.e., 𝑛+1 = 𝜏𝑖𝑗 𝜏𝑖𝑗 𝑛 + Δ𝜏𝑖𝑗 𝑛+1 2⁄ . The desired Cauchy stress at 𝑛 + 1 can now be found 𝑛+1 = 𝑅𝑖𝑘 𝜎𝑖𝑗 𝑛+1𝑅𝑗𝑙 𝑛+1𝜏𝑘𝑙 𝑛+1. (21.24) (21.25) (21.26) (21.27) (21.28) Because we evaluate our constitutive models in the rotated configuration, we avoid the need to transform history variables such as the back stress that arises in kinematic hardening. In the computation of 𝐑, Taylor and Flanagan [1989] did an incremental update in contrast with the direct polar decomposition used in the NIKE3D code. Following their notation the algorithm is given by. LS-DYNA Theory Manual Stress Update Overview 𝑧𝑖 = 𝑒𝑖𝑗𝑘𝑉𝑗𝑚𝜀̇𝑚𝑘, 𝜛𝑖 = 𝑒𝑖𝑗𝑘𝜔𝑗𝑘 − 2[𝑉𝑖𝑗 − 𝛿𝑖𝑗𝑉𝑘𝑘] −1 𝑧𝑗, 𝛺𝑖𝑗 = 𝑒𝑖𝑗𝑘𝜛𝑘, 𝛥𝑡 𝛺𝑖𝑘) 𝑅𝑘𝑗 𝛥𝑡 𝑛+1 = (𝛿𝑖𝑘 + (𝛿𝑖𝑘 − 𝑉̇𝑖𝑗 = (𝜀̇𝑖𝑘 + 𝜔𝑖𝑘)𝑉𝑘𝑗 − 𝑉𝑖𝑘𝛺𝑘𝑗, 𝑛 + 𝛥𝑡𝑉̇𝑖𝑗. 𝑉𝑖𝑗 𝑛+1 = 𝑉𝑖𝑗 𝑛 , 𝛺𝑖𝑘) 𝑅𝑘𝑗 (21.29) We have adopted the PRONTO3D approach in LS-DYNA due to numerical difficulties with the polar decomposition in NIKE3D. We believe the PRONTO3D approach is reliable. Several disadvantages of the PRONTO3D approach include 300+ operations (at least that is the number we got), the requirement of 15 additional variables per integration point, and if we rezone the material in the future the initial geometry will need to be remapped and the 15 variables initialized. 21.4 Elastoplastic Materials At low stress levels in elastoplastic materials the stresses, 𝜎𝑖𝑗, depends only on the state of strain; however, above a certain stress level, called the yield stress, 𝜎𝑦(𝑎𝑖), Initial uniaxial yield point σ y0 y = σ experimental curve y(ai) L0 plastic strain ε = ln(L/L0) σ = P/A elastic strain Figure 21.1. The uniaxial tension test demonstrates plastic behavior. Stress Update Overview LS-DYNA Theory Manual yield surface defined by F(δ ij, k) 1 = σ 2 = σ deviatoria plane yield curve = intersection of the deviatoric plane with the yield surface The yield surface in principal stress space in pressure Figure 21.2. independent. nonrecoverable plastic deformations are obtained. The yield stress changes with increasing plastic deformations, which are measured by internal variables, 𝑎𝑖. In the uniaxial tension test, a curve like that in Figure 21.1 is generated where logrithmic uniaxial strain is plotted against the uniaxial true stress which is defined as the applied load 𝑃 divided by the actual cross-sectional area, 𝐴. For the simple von Mises plasticity models the yield stress is pressure independent and the yield surface is a cylinder in principal stress space as shown in Figure 21.2. With isotropic hardening the diameter of the cylinder grows but the shape remains circular. In kinematic hardening the diameter may remain constant but will translate in the plane as a function of the plastic strain tensor, See Figure 21.3. The equation describing the pressure independent yield surface, 𝐹, is a function of the deviatoric stress tensor, 𝑠𝑖𝑗, of a form given in Equation (1.30). 𝐹(𝑠𝑖𝑗, 𝑎𝑖) = 𝑓 (𝑠𝑖𝑗) − 𝜎𝑦(𝑎𝑖) = 0, (21.30) 𝑓 (𝑠𝑖𝑗) = determines the shape, 𝜎𝑦(𝑎𝑖) = determines the translation and size. The existence of a potential function, 𝑔, called the plastic potential, is assumed Stability and uniqueness require that: 𝑔 = 𝑔(𝑠𝑖𝑗). p = 𝜆 𝑑𝜀𝑖𝑗 𝜕𝑔 𝜕𝑠𝑖𝑗 , (21.31) (21.32) LS-DYNA Theory Manual Stress Update Overview initial yield curve in the deviatoric plane current yield surface Figure 21.3. With kinematic hardening the yield surface may shift as a function of plastic strain. where 𝜆 is a proportionality constant. As depicted in Figure 21.5 the plastic strain increments 𝑑𝜀𝑖𝑗 p are normal to the plastic potential function. This is the normality rule of plasticity. The plastic potential 𝑔 is identical with the yield condition 𝐹(𝑠𝑖𝑗) Hence: 𝑔 ≡ 𝐹. 𝑝 = 𝜆 𝑑𝜀𝑖𝑗 𝜕𝑓 𝜕𝑠𝑖𝑗 = 𝜆 grad𝑓 and the stress increments 𝑑𝑠𝑖𝑗 are normal to the plastic flow ∂𝑔 ∂s𝑖𝑗 . (21.33) (21.34) Post-yielding behavior from uniaxial tension tests typically show the following behaviors illustrated in Figure 21.4: The behavior of these hardening laws are characterized in Table 1.1. below. Although LS-DYNA permits softening to be defined and used, such softening behavior will result in strain localization and nonconvergence with mesh refinement. Stress Update Overview LS-DYNA Theory Manual (cid:1) (cid:1) (cid:1)0 hardening (cid:1) (cid:1) (cid:1)0 (cid:2) (cid:1) (cid:1) (cid:1)0 ideal (cid:2) (cid:2) softening Figure 21.4. Hardening, ideal, and softening plasticity models. Hardening Ideal Softening Behavior Stability Uniqueness Applications 𝜎𝑦(𝑎𝑖) monotonic increasing yes yes is 𝜎𝑦(𝑎𝑖) is constant is 𝜎𝑦(𝑎𝑖) monotonic decreasing yes yes No No metals, concrete, with deformations rock small crude idealization for steel, plastics, etc. dense sand, concrete with large deformations Table 21.1. Plastic hardening, ideal plasticity, and softening. 21.5 Hyperelastic Materials Stresses independent; for elastic and hyperelastic materials are path consequently, the stress update is not computed incrementally. The methods described here are well known and the reader is referred to Green and Adkins [1970] and Ogden [1984] for more details. A retangular cartesian coordinate system is used so that the covariant and con- travariant metric tensors in the reference (undeformed) and deformed configuration are: 𝐺𝑖𝑗 = 𝑔𝑖𝑗 = 𝑔𝑖𝑗 = 𝛿𝑖𝑗, 𝜕𝑥𝑘 𝜕𝑥𝑘 𝜕𝑋𝑗 𝜕𝑋𝑖 𝜕𝑋𝑗 𝜕𝑋𝑖 𝜕𝑥𝑘 𝜕𝑥𝑘 𝐺𝑖𝑗 = . , (21.35) LS-DYNA Theory Manual Stress Update Overview The Green-St. Venant strain tensor and the principal strain invariants are defined as 𝛾𝑖𝑗 = (𝐺𝑖𝑗 − 𝛿𝑖𝑗), 𝐼1 = 𝛿𝑖𝑗𝐺𝑖𝑗, 𝐼2 = 𝐼3 = det(𝐺𝑖𝑗), (𝛿𝑖𝑟𝛿𝑗𝑠𝐺𝑟𝑖𝐺𝑠𝑗 − 𝛿𝑖𝑟𝛿𝑗𝑠𝐺𝑖𝑗𝐺𝑟𝑠), (21.36) (21.37) For a compressible elastic material the existence of a strain energy functional, 𝑊, is assumed 𝑊 = 𝑊(𝐼1, 𝐼2, 𝐼3), (21.38) which defines the energy per unit undeformed volume. The stress measured in the deformed configuration is given as [Green and Adkins, 1970]: (cid:4) (cid:1)(cid:2)(cid:3) (cid:1) Figure 21.5. The plastic strain is normal to the yield surface. 𝑠𝑖𝑗 = 𝛷𝑔𝑖𝑗 + 𝛹𝐵𝑖𝑗 + 𝑝𝐺𝑖𝑗, where , 𝛷 = 𝛹 = √𝐼3 𝜕𝑊 𝜕𝐼1 𝜕𝑊 𝜕𝐼2 𝜕𝑊 𝑝 = 2√𝐼3 𝜕𝐼3 𝐵𝑖𝑗 = 𝐼1𝛿𝑖𝑗 − 𝛿𝑖𝑟𝛿𝑗𝑠𝐺𝑟𝑠. √𝐼3 , , (21.39) (21.40) Stress Update Overview LS-DYNA Theory Manual This stress is related to the second Piola-Kirchhoff stress tensor: Second Piola-Kirchhoff stresses are transformed to physical (Cauchy) stresses according to the relationship: 𝑆𝑖𝑗 = 𝑠𝑖𝑗√𝐼3. (21.41) 𝜎𝑖𝑗 = 𝜌0 𝜕𝑥𝑖 𝜕𝑋𝑘 𝜕𝑥𝑗 𝜕𝑋𝑙 𝑆𝑘𝑙. (21.42) 21.6 Layered Composites The composite models for shell elements in LS-DYNA include models for elastic behavior and inelastic behavior. The approach used here for updating the stresses also applies to the airbag fabric model. To allow for an arbitrary orientation of the shell elements within the finite element mesh, each ply in the composite has a unique orientation angle, 𝛽, which measures the offset from some reference in the element. Each integration point through the shell thickness, typically though not limited to one point per ply, requires the definition of 𝛽 at that point. The reference is determined by the angle 𝛹, which can be defined for each element on the element card, and is measured from the 1-2 element side. Figures 21.6 and 21.7 depict these angles. We update the stresses in the shell in the local shell coordinate system which is defined by the 1-2 element side and the cross product of the diagonals. Thus to transform the stress tensor into local system determined by the fiber directions entails a transformation that takes place in the plane of the shell. In the implementation of the material model we first transform the Cauchy stress and velocity strain tensor 𝑑𝑖𝑗into the coordinate system of the material denoted by the subscript L 𝛔L = 𝛔L = 𝐪T𝛔𝐪, 𝐪L = 𝐪T𝐝𝐪, 𝜎11 𝜎12 𝜎13 ⎥⎤ , ⎢⎡ 𝜎21 𝜎22 𝜎23 𝜎32 𝜎32 𝜎33⎦ ⎣ 𝑑12 𝑑11 ⎡ 𝑑22 𝑑21 ⎢ 𝑑32 𝑑32 ⎣ 𝑑13 ⎤ 𝑑23 , ⎥ 𝑑33⎦ 𝛆L = (21.43) LS-DYNA Theory Manual Stress Update Overview θ = ψ+β Figure 21.7. A multi-layer laminate can be defined. The angle βi is defined for the ith lamina. The Arabic subscripts on the stress and strain (𝛔 and 𝛆) are used to indicate the principal material directions where 1 indicates the fiber direction and 2 indicates the transverse fiber direction (in the plane). The orthogonal 3 × 3 transformation matrix is given by 𝐪 = cos𝜃 −sin𝜃 ⎢⎡ cos𝜃 sin𝜃 ⎣ ⎥⎤. 1⎦ (21.44) In shell theory we assume a plane stress condition, i.e., that the normal stress, 𝜎33, to the mid-surface is zero. We can now incrementally update the stress state in the material coordinates 𝑛+1 = 𝛔L 𝛔L 𝑛 + Δ𝛔L 𝑛+1 2⁄ , (21.45) where for an elastic material n4 n2 n3 n1 Figure 21.6. Orientation of material directions relative to the 1-2 side. Stress Update Overview LS-DYNA Theory Manual 𝑛+1 2⁄ Δ𝛔L = Δ𝜎11 ⎤ ⎡ Δ𝜎22 ⎥ ⎢ ⎥ ⎢ Δ𝜎12 ⎥ ⎢ Δ𝜎23 ⎥ ⎢ Δ𝜎31⎦ ⎣ = 𝑄11 𝑄12 ⎡ 𝑄12 𝑄22 ⎢ ⎢ ⎢ ⎢ ⎣ 𝑄44 𝑄55 ⎤ ⎥ ⎥ ⎥ ⎥ 𝑄66⎦ 𝑑11 ⎤ 𝑑22 ⎥ ⎥ 𝑑12 ⎥ 𝑑23 ⎥ 𝑑31⎦ ⎡ ⎢ ⎢ ⎢ ⎢ ⎣ Δ𝑡. (21.46) The terms 𝑄𝑖𝑗 are referred to as reduced components of the lamina and are defined as , , , (21.47) 𝑄11 = 𝑄22 = 𝑄12 = 𝐸11 1 − 𝜈12𝜈21 𝐸22 1 − 𝜈12𝜈21 𝜈12𝐸11 1 − 𝜈12𝜈21 𝑄44 = 𝐺12, 𝑄55 = 𝐺23, 𝑄66 = 𝐺31. Because of the symmetry properties, 𝐸𝑗𝑗 𝐸𝑖𝑖 where 𝜈𝑖𝑗 is Poisson’s ratio for the transverse strain in jth direction for the material undergoing stress in the ith-direction, 𝐸𝑖𝑗 are the Young’s modulii in the ith direction, and 𝐺𝑖𝑗 are the shear modulii. 𝜈𝑗𝑖 = 𝜈𝑖𝑗 (21.48) , After completion of the stress update we transform the stresses back into the local shell coordinate system. 𝛔 = 𝐪𝛔L𝐪T. (21.49) 21.7 Constraints on Orthotropic Elastic Constants The inverse of the constitutive matrix 𝐂l is generally defined in terms of the local material axes for an orthotropic material is given in terms of the nine independent elastic constants as LS-DYNA Theory Manual Stress Update Overview −1 = 𝐂l 𝐸 11 𝜐 12 𝐸 11 𝜐 13 𝐸 11 − − − 𝜐 21 𝐸 22 𝐸 22 𝜐 23 𝐸 22 − − − 𝜐 31 𝐸 33 𝜐 32 𝐸 33 𝐸 33 ⎡ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎣ 𝐺12 𝐺23 ⎤ ⎥ ⎥ ⎥ ⎥ ⎥ ⎥ ⎥ ⎥ . ⎥ ⎥ ⎥ ⎥ ⎥ ⎥ ⎥ ⎥ 𝐺31⎦ (21.50) As discussed by Jones [1975], the constants for a thermodynamically stable material must satisfy the following inequalities: 𝐸1, 𝐸2, 𝐸3, 𝐺12, 𝐺23, 𝐺31 > 0, 𝐶11,𝐶22, 𝐶33, 𝐶44, 𝐶55, 𝐶66 > 0, (1 − 𝜈23𝜈32), (1 − 𝜈13𝜈31), 1 − 𝜈12𝜈21 − 𝜈23𝜈32 − 𝜈31𝜈13 − 2𝜈21𝜈32𝜈13 > 0. (1 − 𝜈12𝜈21) > 0, Using Equation (21.48) and (21.51) leads to: |𝜈21| < ( |𝜈12| < ( ∣𝜈32∣ < ( ∣𝜈23∣ < ( ∣𝜈13∣ < ( ∣𝜈31∣ < ( 2⁄ ) 2⁄ ) 2⁄ ) 𝐸22 𝐸11 𝐸33 𝐸22 𝐸11 𝐸33 , , 2⁄ ) 2⁄ ) ) 2⁄ . 𝐸11 𝐸22 𝐸22 𝐸33 𝐸33 𝐸11 (21.51) (21.52) 21.8 Local Material Coordinate Systems in Solid Elements In solid elements there is a number of different ways of defining a local coordinate system. Perhaps the most general is by defining a triad for each element that is oriented in the local material directions, See Figure 21.8. In this approach two vectors 𝐚 and 𝐝 are defined. The local 𝐜 direction is found from the cross product, 𝐜 = 𝐚 × 𝐝, the local 𝐛 direction is the cross product 𝐛 = 𝐜 × 𝐚. This triad is stored as history data at each integration point. Stress Update Overview LS-DYNA Theory Manual Figure 21.8. Local material directions are defined by a triad which can be input for each solid element. The biggest concern when dealing with local material directions is that the results are not invariant with element numbering since the orientation of the local triad is fixed with respect to the base of the brick element, nodes 1-4, in Figure 21.9. For Hyperelastic materials where the stress tensor is computed in the initial configuration, this is not a problem, but for materials like the honeycomb foams, the local directions can change due to element distortion causing relative movement of nodes 1-4. In honeycomb foams we assume that the material directions are orthogonal in the deformed configuration since the stress update is performed in the deformed configuration. 21.9 General Erosion Criteria for Solid Elements Several erosion criteria are available that are independent of the material models. Each one is applied independently, and once any one of them is satisfied, the element is deleted from the calculation. The criteria for failure are: • 𝑃 ≥ 𝑃min where P is the pressure (positive in compression), and 𝑃min is the pressure at failure. • 𝜎1 ≥ 𝜎max, where 𝜎1 is the maximum principal stress, and 𝜎max is the principal stress at failure. • √3 ′ 𝜎𝑖j 2 𝜎𝑖𝑗 ′ ≥ 𝜎̅̅̅̅̅max, where 𝜎𝑖𝑗 equivalent stress at failure. ′ are the deviatoric stress components, and 𝜎̅̅̅̅̅max is the • 𝜀1 ≥ 𝜀max, where 𝜀1 is the maximum principal strain, and 𝜀max is the principal strain at failure. • 𝛾1 ≥ 𝛾max, where 𝛾1 is the shear strain, and 𝛾max is the shear strain at failure. • The Tuler-Butcher criterion, LS-DYNA Theory Manual Stress Update Overview Figure 21.9. The orientation of the triad for the local material directions is stored relative to the base of the solid element. The base is defined by nodes 1- 4 of the element connectivity. ∫ [max(0, 𝜎1 − 𝜎0)]2𝑑𝑡 ≥ 𝐾f, (21.53) where 𝜎1 is the maximum principal stress, 𝜎0 is a specified threshold stress, 𝜎1 ≥ 𝜎0 ≥ 0, and 𝐾f is the stress impulse for failure. Stress values below the threshold value are too low to cause fracture even for very long duration loadings. Typical constants are given in Table 1.2 below [Rajendran, 1989]. These failure models apply to solid elements with one point integration in 2 and 3 dimensions. Material 1020 Steel OFHC Copper C1008 HY100 7039-T64 𝜎0 (Kbar) 10.0 3.60 14.0 15.7 8.60 2 2 2 2 2 12.5 10.0 0.38 61.0 3.00 Table 21.2. Typical constants for the Tuler-Bucher criterion. 21.10 Strain Output to the LS-DYNA Database The strain tensors that are output to the LS-DYNA database from the solid, shell, and beam elements are integrated in time. These strains are similar to the logarithmic strain measure and are based on an integration of the strain rate tensor. Admittedly, Stress Update Overview LS-DYNA Theory Manual the shear strain components do not integrate as logarithmic strain measures, but in spite of this, we have found that the strains output from LS-DYNA are far more useful than those computed in LS-DYNA. The time integration of the strain tensor in LS-DYNA maintains objectivity in the sense that rigid body motions do not cause spurious straining. Recall, the spin tensor and strain rate tensor, Equations (21.3) and (21.5), respectively: 𝜔𝑖𝑗 = 𝜀̇𝑖𝑗 = ( 𝜕𝑣𝑖 𝜕𝑥𝑗 − 𝜕𝑣𝑗 𝜕𝑥𝑖 ), ( 𝜕𝑣𝑖 𝜕𝑥𝑗 + 𝜕𝑣𝑗 𝜕𝑥𝑖 ). In updating the strains from time 𝑛 to 𝑛 + 1, the following formula is used: 𝑛+1 = 𝜀𝑖𝑗 𝜀𝑖𝑗 𝑛 + 𝜌𝑖𝑗 𝑛 + 𝜀̇𝑖𝑗 𝑛+1 2⁄ Δ𝑡𝑛+1 2⁄ , (21.54) (21.55) (21.56) 𝑛 gives the rotational correction that transforms the strain tensor at time 𝑡𝑛 into where 𝜌𝑖𝑗 the configuration at 𝑡𝑛 + 1 𝑛 = (𝜀𝑖𝑝 𝜌𝑖𝑗 𝑛 𝜔𝑝𝑗 𝑛+1 2⁄ 𝑛+1 + 𝜀𝑗𝑝 𝑛 𝜔𝑝𝑖 2⁄ ) Δ𝑡𝑛+1 2⁄ . (21.57) For shell elements we integrate the strain tensor at the inner and outer integration points and output two tensors per element. When the mid surface strains are plotted in LS-PREPOST, these are the average values. 21.11 Strain Rate Effects in Material Models In a constitutive modeling context, the term rate effects is used to indicate that the material response depends on the (time) rate of a certain quantity, here called 𝑒 for the sake of generality. This quantity is usually some kind of strain measure, and an example is when the stress depends on the rate of strain. In explicit simulations, high frequency strain content yields a very noisy strain rate and calls for some kind of smoothing before being used in the stress calculations. This section presents three of the common ways to do this averaging and that are used frequently in the material models. 21.11.1 Running N-average option One option is to do a running average of current and previous strain rates. With this option the rate 𝑒 ̇ of a quantity 𝑒 is averaged according to the following algorithm LS-DYNA Theory Manual Stress Update Overview ̇ = unfiltered rate (raw data) 𝑒 ̃ 𝑒 ̃ 𝑒 ̇𝑛 = ̇+ ∑ 𝑛−1 𝑖=𝑛−𝑁+1 𝑒 ̇𝑖 𝑒 ̇ = 𝑒 ̇𝑛 = rate used in material routine (21.1) (21.2) (21.3) In these equations, the subscript denotes stored history variables necessary for computing the running average strain rates and n denotes the current cycle number. This requires storage of 𝑁 − 1 history variables, for most materials 𝑁 = 12. 21.11.2 Last N-average option The second option is to compute the rate as the average of the last 𝑁 computed rates. Here the rate is evaluated according to 𝑒 ̃ ̇ = unfiltered rate (raw data) ̇ 𝑒 ̇𝑛 = 𝑒 ̃ 𝑒 ̇ = ∑ 𝑖=𝑛−𝑁+1 𝑒 ̇𝑖 = rate used in material routine (21.4) (21.5) (21.6) As for the running average option, the subscript denotes stored history variables necessary for computing the running average strain rates and n is the cycle number. This also requires storage of 𝑁 − 1 history variables, for most materials 𝑁 = 12. 21.11.3 Averaging over a fixed amount of time 𝑻 This option was introduced in an attempt to suppress the time step dependence as much as possible. With this option we use 𝑁 history variables to store the approximate values of the quantity of interest from the time 𝑡𝑛 − 𝑇 to current time 𝑡𝑛. That is, we set 𝑒𝑛−𝑖 = 𝑒𝑛 (𝑡𝑛 − 𝑖𝑇 𝑁 − 1 ) , 𝑖 = 0, … , 𝑁 − 1 (21.7) Here 𝑒𝑛(𝑡) is an approximate function of the function of interest, 𝑒(𝑡), and will be given more specifically below. Assuming 𝑒𝑛(𝑡) is known, the rate used in the material routine in cycle 𝑛 is simply 𝑒 ̇ = 𝑒𝑛 − 𝑒𝑛−𝑁+1 = rate used in material routine (21.8) For the update of history variables we assume that the 𝑁 points in (21.7) together with the newly calculated quantity (raw data) at 𝑡𝑛+1 = 𝑡 + ∆𝑡, (21.9) completely define the function 𝑒𝑛(𝑡) from time 𝑡𝑛 − 𝑇 to time 𝑡𝑛+1 by linear interpolation between each control point. That is, the function 𝑒𝑛(𝑡) is extended to time 𝑡𝑛+1 by the new value, 𝑒𝑛+1 = 𝑒(𝑡𝑛+1), 𝑒𝑛(𝑡𝑛+1) = 𝑒𝑛+1. (21.10) Stress Update Overview LS-DYNA Theory Manual This function is illustrated in the figure below by the dashed line and red control points. The updated set of history variables are 𝑒𝑛+1−𝑖 = 𝑒𝑛 (𝑡𝑛+1 − 𝑖𝑇 𝑁 − 1 ) , 𝑖 = 0, … , 𝑁 − 1, (21.11) and these updated points define a new approximate function 𝑒𝑛+1(𝑡), again by linear interpolation between the control points. In Figure 21.1, the updated function is illustrated by the solid line and blue control points, note that the last point is in fact both red and blue since 𝑒𝑛(𝑡𝑛+1) = 𝑒𝑛+1(𝑡𝑛+1) = 𝑒𝑛+1. In sum, the function used for calculated the effective rate is completely redefined between steps. For a time step ∆𝑡 that is greater than or approximately equal to 𝑇/(𝑁 − 1), this option is more or less exactly the average rate from 𝑡 − 𝑇 to 𝑡. For smaller time steps (which is usually the case in explicit analysis) the previous values are in practice smoothed out since only 𝑁 variables are available for storing this time history. That is, the high frequency content of the history is lost and this could be an interesting alternative to the previous two options that are otherwise commonly used for these types of situations. 𝑒 Control points and function 𝑒𝑛(𝑡) Control points and function 𝑒𝑛+1(𝑡) 𝑒𝑛+1 = 𝑒(𝑡𝑛+1) 𝑡𝑛 𝑡𝑛+1 𝑡𝑛 − 𝑇 Figure 21.1. Illustration of control point update for 𝑁 = 4 21.12 Algorithmic Consistent Tangent Modulus for Plasticity For materials used in implicit analysis, the tangent modulus is needed for global assembly of the stiffness matrix. In particular, the softening effect in elastic-plastic materials must be predicted when in a plastic state. The following is a derivation of the tangent modulus that is consistent with the algorithmic stress update, meaning that it provides the exact variation of the stress with respect to the rate of deformation. We restrict ourselves to the plane stress update, as the full 3D situation is less complicated. LS-DYNA Theory Manual Stress Update Overview As a prerequisite, the algorithmic stress update must be established mathematically. For this, and the rest of this section, we introduce the variables Δ𝝈 − stress increment, excluding through thickness stress ∆𝜎3 ∆𝜀3 − through thickness strain increment ∆𝜀𝑝 − plastic strain increment ∆𝜶 − back stress increment, full tensor to be sought, the parameters 𝑪 − 3𝐷 elastic tensor Δ𝜺 − strain increment, excluding through thickness strain ∆𝜀3 𝑷 − projection from 3D to plane stress space 𝒑𝑇 − projection from 3D to out of plane space that are given, and the functions 𝑓 (𝑷𝑇Δ𝝈 − Δ𝜶, ∆𝜀𝑝) − yield function 𝑔(𝑷𝑇Δ𝝈 − Δ𝜶, ∆𝜀𝑝) − plastic flow function ℎ(𝑷𝑇Δ𝝈 − Δ𝜶, ∆𝜀𝑝) − back stress potential that define the plasticity. This theory thus incorporates full anisotropy as well as non- associative plasticity. The stress update can be summarized by the combination of four equations; the stress update Δ𝝈 = 𝑷𝑪 ⎜⎛𝑷𝑇∆𝜺 + 𝒑∆𝜀3 − { ⎝ } 𝜕𝑔 𝜕𝝈 ∆𝜀𝑝 ⎟⎞, ⎠ (21.12) the yield condition 𝑓 = 𝜎(𝑷𝑇(𝝈0 + Δ𝝈) − (𝜶0 + Δ𝜶)) − 𝜎𝑌(𝜀0 + ∆𝜀𝑝) = 0, (21.13) the evolution of back stress Δ𝜶 = { } 𝜕ℎ 𝜕𝝈 ∆𝜀𝑝, and the plane stress condition ∆𝜎3 = 𝒑𝑇𝑪 ⎜⎛𝑷𝑇∆𝜺 + 𝒑∆𝜀3 − { ⎝ } ∆𝜀𝑝 𝜕𝑔 𝜕𝝈 ⎟⎞ = 0. ⎠ (21.14) (21.15) The expression for 𝑓 in (21.13) is in terms of effective stress 𝜎 equals the yield stress 𝜎𝑌, but the theory is not restricted to this setting. It is assumed that the stress 𝝈0, back stress 𝜶0 Stress Update Overview LS-DYNA Theory Manual and the plastic strain 𝜀0 in the previous step fulfils the corresponding conditions (21.12), (21.13), (21.14) and (21.15) with respect to the state at that time, possibly with inequality in (21.13). Taking the variation of these four equations results in δΔ𝝈 = 𝑷𝑪 } δ∆𝜀𝑝 − 𝜕𝑔 𝜕𝝈 𝜕2𝑔 𝜕𝝈2 (𝑷𝑇δΔ𝝈 − δΔ𝜶)∆𝜀𝑝 ⎜⎛𝑷𝑇δ∆𝜺 + 𝒑δ∆𝜀3 − { ⎝ − 𝜕2𝑔 𝜕𝝈𝜕𝜀𝑝 δΔ𝜀𝑝∆𝜀𝑝 ⎟⎞, ⎠ (𝑷𝑇δΔ𝝈 − δΔ𝜶) + 𝜕𝑓 𝜕𝜀𝑝 δΔ𝜀𝑝 = 0, 𝜕𝑓 𝜕𝝈 δΔ𝜶 = { 𝜕ℎ 𝜕𝝈 } δ∆𝜀𝑝 + 𝜕2ℎ 𝜕𝝈2 (𝑷𝑇δΔ𝝈 − δΔ𝜶)∆𝜀𝑝 + 𝜕ℎ 𝜕𝝈𝜕𝜀𝑝 δ∆𝜀𝑝∆𝜀𝑝, (21.16) (21.17) (21.18) 𝒑𝑇𝑪 ⎜⎛𝑷𝑇δ∆𝜺 + 𝒑δ∆𝜀3 − { ⎝ = 0. } δ∆𝜀𝑝 − 𝜕𝑔 𝜕𝝈 𝜕2𝑔 𝜕𝝈2 (𝑷𝑇δΔ𝝈 − δΔ𝜶)∆𝜀𝑝 − 𝜕2𝑔 𝜕𝝈𝜕𝜀𝑝 δΔ𝜀𝑝∆𝜀𝑝 ⎟⎞ ⎠ (21.19) Solving (21.16) and (21.18) for 𝑷𝑇δΔ𝝈 − δΔ𝜶 results in 𝑷𝑇δΔ𝝈 − δΔ𝜶 = 𝑨−1𝑷𝑇𝑷𝑪𝑷𝑇δ∆𝜺 + 𝑨−1𝑷𝑇𝑷𝑪𝒑δ∆𝜀3 − 𝑨−1𝑭δ∆𝜀𝑝 (21.20) where 𝑨 = 𝑰 + 𝑷𝑇𝑷𝑪 𝜕2ℎ 𝜕𝝈2 ∆𝜀𝑝 } + 𝜕𝑔 𝜕𝝈 𝜕2𝑔 𝜕𝝈2 ∆𝜀𝑝 + 𝜕2𝑔 𝜕𝝈𝜕𝜀𝑝 𝜕2ℎ 𝜕𝝈𝜕𝜀𝑝 𝑭 = 𝑷𝑇𝑷𝑪𝑮 + 𝑯. 𝜕ℎ 𝜕𝝈 } + 𝑮 = { 𝑯 = { ∆𝜀𝑝 ∆𝜀𝑝 (21.21) Inserting (21.20) into (21.17) and (21.19) results in a system of equations 𝒑𝑇𝑬𝑪𝒑 𝑨−1𝑷𝑇𝑷𝑪𝒑 ⎜⎜⎜⎜⎛ ⎝ − 𝜕𝑓 𝜕𝝈 𝒑𝑇𝑳 𝑨−1𝑭 − 𝜕𝑓 𝜕𝝈 ⎟⎟⎟⎟⎞ 𝜕𝑓 𝜕𝜀𝑝⎠ ( δ∆𝜀3 δ∆𝜀𝑝 ) = −𝒑𝑇𝑬 ⎟⎟⎟⎞ 𝑨−1𝑷𝑇𝑷⎠ ⎜⎜⎜⎛ ⎝ 𝜕𝑓 𝜕𝝈 𝑪𝑷𝑇δ∆𝜺. (21.22) where LS-DYNA Theory Manual Stress Update Overview Solving (21.22) results in and 𝜕2𝑔 𝜕𝝈2 𝑨−1𝑷𝑇𝑷∆𝜀𝑝 𝑬 = 𝑰 − 𝑪 𝜕2𝑔 𝜕𝝈2 𝑨−1𝑭∆𝜀𝑝 − 𝑮). 𝑳 = 𝑪 ( δ∆𝜀3 = 𝒂3 𝑇𝑩𝑪𝑷𝑇δ∆𝜺 δ∆𝜀𝑝 = 𝒂𝑝 𝑇𝑩𝑪𝑷𝑇δ∆𝜺 (21.23) (21.24) (21.25) 𝑇 and 𝒂𝑝 𝑇 are rows in the inverse of the system matrix in (21.22) and 𝑩 can be where 𝒂3 identified on the right-hand side of the same equation. Inserting (21.24) and (21.25) into (21.20) results in δΔ𝝈 = 𝑷(𝑬 + 𝑬𝑪𝒑𝒂3 𝑇𝑩 + 𝑳𝒂𝑝 𝑇𝑩)𝑪𝑷𝑇δ∆𝜺 from which the consistent tangent matrix can be identified as 𝑫 = 𝑷(𝑬 + 𝑬𝑪𝒑𝒂3 𝑇𝑩 + 𝑳𝒂𝑝 𝑇𝑩)𝑪𝑷𝑇. (21.26) (21.27) Even though the involved expressions seem complicated, many expressions are repeated, and they simplify quite a bit when considering special cases. As an example, consider isotropic von Mises plasticity with linear hardening and back stress (mixed formulation) for which we have 𝑓 = 𝑔 = 𝜎 − 𝜎𝑌 − 𝛽𝐻𝜀𝑝 ℎ = (1 − 𝛽)𝐻𝑓 (21.28) where 𝜎 = √3 Then 2 𝒔𝑇𝒔 and 𝒔 is the deviatoric stress, including subtraction of back stress 𝜶. 𝜕𝑓 𝜕𝝈 𝜕ℎ 𝜕𝝈 = = = 𝜕𝑔 𝜕𝝈 2𝜎 (1 − 𝛽)𝐻 𝒔𝑇 𝒔𝑇 and (𝑰𝑑𝑒𝑣 − 𝜕2𝑔 𝜕𝝈2 = 2𝜎 (1 − 𝛽)𝐻 𝜕2ℎ 𝜕𝝈2 = 2𝜎 2 𝒔𝒔𝑇) 2𝜎 2 𝒔𝒔𝑇) (𝑰𝑑𝑒𝑣 − (21.29) (21.30) Stress Update Overview LS-DYNA Theory Manual If the elastic matrix 𝑪 is isotropic, then we have and 𝜕𝑓 𝜕𝝈 𝑪 = 3𝐺 𝒔𝑇 𝜕2𝑔 𝜕𝝈2 = 3𝐺 (𝑰𝑑𝑒𝑣 − 2𝜎 2 𝒔𝒔𝑇) (21.31) (21.32) with 𝐺 being the shear modulus, resulting in an 𝑨 matrix that is invertible on closed form. We also have 𝜕2𝑔 𝜕𝝈𝜕𝜀𝑝 = 𝜕2ℎ 𝜕𝝈𝜕𝜀𝑝 = 𝟎. (21.33) In 3D constitutive laws, 𝑷 = 𝑰 and 𝒑 = 𝟎, so the system (21.22) reduces to a scalar 𝑇 = 𝟎 in (21.27), and so on, so the implementation is very much equation with 𝒂3 tractable. LS-DYNA Theory Manual Material Models 22 Material Models LS-DYNA accepts a wide range of material and equation of state models, each with a unique number of history variables. Approximately 150 material models are implemented, and space has been allotted for up to 10 user-specified models. Elastic Orthotropic Elastic Kinematic/Isotropic Elastic-Plastic Thermo-Elastic-Plastic Soil and Crushable/Non-crushable Foam Viscoelastic Blatz - Ko Rubber High Explosive Burn Null Hydrodynamics Isotropic-Elastic-Plastic-Hydrodynamic Temperature Dependent, Elastoplastic, Hydrodynamic Isotropic-Elastic-Plastic Elastic-Plastic with Failure Model Soil and Crushable Foam with Failure Model Johnson/Cook Strain and Temperature Sensitive Plasticity Pseudo TENSOR Concrete/Geological Model Isotropic Elastic-Plastic Oriented Crack Model Power Law Isotropic Plasticity Strain Rate Dependent Isotropic Plasticity Rigid Thermal Orthotropic Elastic Composite Damage Model Thermal Orthotropic Elastic with 12 Curves Piecewise Linear Isotropic Plasticity Inviscid Two Invariant Geologic Cap Model 1 2 3 4 5 6 7 8 9 10 11 12 13 14 15 16 17 18 19 20 21 22 23 24 25 26 Metallic Honeycomb Material Models LS-DYNA Theory Manual Planar Anisotropic Plasticity Model Strain Rate Dependent Plasticity with Size Dependent Failure Temperature and Rate Dependent Plasticity Sandia’s Damage Model Low Density Closed Cell Polyurethane Foam Compressible Mooney-Rivlin Rubber Resultant Plasticity Force Limited Resultant Formulation Closed-Form Update Shell Plasticity Slightly Compressible Rubber Model Laminated Glass Model Barlat’s Anisotropic Plasticity Model Fabric Kinematic/Isotropic Elastic-Plastic Green-Naghdi Rate Barlat’s 3-Parameter Plasticity Model Transversely Anisotropic Elastic-Plastic Blatz-Ko Compressible Foam Transversely Anisotropic Elastic-Plastic with FLD 27 28 29 30 31 32 33 34 35 36 37 38 39 40 Nonlinear Elastic Orthotropic Material 41-50 User Defined Material Models 42 48 51 52 53 54-55 Composite Damage Model 57 Low Density Urethane Foam 58 Laminated Composite Fabric 59 Composite Failure Elastic with Viscosity 60 61 Maxwell/Kelvin Viscoelastic 62 63 64 65 Modified Zerilli/Armstrong 66 67 Nonlinear Stiffness/Viscous 3D Discrete Beam 68 Nonlinear Plastic/Linear Viscous 3D Discrete Beam 69 Side Impact Dummy Damper, SID Damper 70 Hydraulic/Gas Damper 71 72 73 74 75 76 General Viscoelastic 77 Hyperviscoelastic Rubber 78 Soil/Concrete 79 Hysteretic Soil 80 Cable Concrete Damage Model Low Density Viscoelastic Foam Elastic Spring for the Discrete Beam Bilkhu/Dubois Foam Model Viscous Foam Isotropic Crushable Foam Strain Rate Sensitive Power-Law Plasticity Linear Stiffness/Linear Viscous 3D Discrete Beam Ramberg-Osgood Plasticity LS-DYNA Theory Manual Material Models Plastic with Damage Isotropic Elastic-Plastic with Anisotropic Damage Fu-Chang’s Foam with Rate Effects Plasticity Polymer 81 82 83 84-85 Winfrith Concrete 84 Winfrith Concrete Reinforcement 86 Orthotropic-Viscoelastic 87 Cellular Rubber 88 MTS Model 89 90 Acoustic Soft Tissue 91 Elastic 6DOF Spring Discrete Beam 93 Inelastic Spring Discrete Beam 94 Inelastic 6DOF Spring Discrete Beam 95 96 Brittle Damage Model 97 General Joint Discrete Beam 100 Spot weld 101 GE Thermoplastics 102 Hyperbolic Sin 103 Anisotropic Viscoplastic 104 Damage 1 105 Damage 2 106 110 111 112 113 114 115 Elastic Creep Model 116 Composite Lay-Up Model 117-118 119 General Spring and Damper Model 120 Gurson Dilational-Plastic Model 120 Gurson Model with Rc-Dc 121 Generalized Nonlinear 1DOF Discrete Beam 122 Hill 3RC 123 Modified Piecewise Linear Plasticity Tension-Compression Plasticity 124 126 Metallic Honeycomb 127 Arruda-Boyce rubber 128 Anisotropic heart tissue 129 Lung tissue 130 Special Orthotropic 131 132 Orthotropic Smeared Crack Elastic Viscoplastic Thermal Johnson-Holmquist Ceramic Model Johnson-Holmquist Concrete Model Finite Elastic Strain Plasticity Transformation Induced Plasticity Layered Linear Plasticity Isotropic Smeared Crack Composite Matrix Material Models LS-DYNA Theory Manual EMMI Barlat YLD2000 Composite MSC Pitzer Crushable Foam Schwer Murray Cap Model 1DOF Generalized Spring FHWA Soil Model 133 134 Viscoelastic Fabric 139 Modified Force Limited 140 Vacuum 141 Rate Sensitive Polymer 142 Transversely Anisotropic Crushable Foam 143 Wood Model 144 145 146 147 148 Gas Mixture 150 CFD 151 154 Deshpande-Fleck Foam 156 Muscle 158 Rate Sensitive Composite Fabric 159 Continuous Surface Cap Model 161-162 163 Modified Crushable Foam 164 Brain Linear Viscoelastic 166 Moment Curvature Beam 169 Arup Adhesive 170 Resultant Anisotropic 175 Viscoelastic Maxwell 176 Quasilinear Viscoelastic 177 Hill Foam 178 Viscoelastic Hill Foam 179 Low Density Synthetic Foam 181 183 184 Cohesive Elastic 185 Cohesive TH 191 Seismic Beam 192 Soil Brick 193 Drucker Prager 194 RC Shear Wall 195 Concrete Beam 196 General Spring Discrete Beam 197 198 Simplified Rubber/Foam Simplified Rubber with Damage Seismic Isolator Jointed Rock LS-DYNA Theory Manual Material Models In the table below, a list of the available material models and the applicable element types are given. Some materials include strain rate sensitivity, failure, equations of state, and thermal effects and this is also noted. General applicability of the materials to certain kinds of behavior is suggested in the last column. Notes: Gn Gen- eral Cm Com- posites Cr Ceram- ics Fl Fluids Fm Foam Gl Glass Hy Hydro- dyn Mt Metal Pl Plastic Rb Rubber Sl Soil/C onc ff - - - ff Y Y Y Y Y Y Y - Gn, Fl Cm, Mt Y Y Y Y Y Y Y Y Y Y Y Y Y Y Y Y Y Cm, Mt, Pl Y Mt, Pl Fm, Sl Rb Rb, Polyurethane Material Title (Anisotropic Elastic Orthotropic Elastic solids) Plastic Kinematic/Isotropic Elastic Plastic Thermal Soil and Foam Linear Viscoelastic Blatz-Ko Rubber Temp. High Explosive Burn Null Material Elastic Plastic Hydro(dynamic) Steinberg: Elastoplastic Isotropic Elastic Plastic Isotropic Elastic Plastic with Failure Soil and Foam with Failure Johnson/Cook Plasticity Model Pseudo TENSOR Geological Model Dependent Y Y Y Y Y Hy Y Y Y Fl, Hy Y Y Hy, Mt Y Y Y Y Hy, Mt Mt Mt Y Y Y Y Y Fm, Sl Y Y Y Y Y Y Y Y Hy, Mt Y Y Y Y Sl 1 2 3 4 5 6 7 8 9 10 11 12 13 14 15 16 Material Models LS-DYNA Theory Manual (Elastoplastic with 17 Oriented Crack Fracture) Power Law Plasticity (Isotropic) Strain Rate Dependent Plasticity 18 19 20 Rigid Y Y Y Hy, Mt, Pl Y Y Y Y Y Y Y Y Y Y Y Y Y Y Mt, Pl Mt, Pl Notes: Gn Gen- eral Cm Com- posites Cr Ce- ramics Fl Fluids Fm Foam Gl Glass Hy Hydro -dyn Mt Metal Pl Plastic Rb Rubber Sl Soil/C onc Material Title ff - - - ff Temperature Dependent Orthotropic Piecewise Linear Plasticity (Isotropic) Inviscid Two Invariant Geologic Cap 21 Orthotropic Thermal (Elastic) 22 Composite Damage 23 24 25 26 Honeycomb 27 Mooney-Rivlin Rubber 28 Resultant Plasticity 29 Force Limited Resultant Formulation 30 Closed Form Update Shell Plasticity Slightly Compressible Rubber 31 Laminated Glass (Composite) 32 Barlat Anisotropic Plasticity 33 Fabric 34 Plastic Green-Naghdi Rate 35 3-Parameter Barlat Plasticity 36 Transversely Anisotropic Elastic Plastic 37 Y Y Y Y Y Y Y Y Y Y Y Y Y Y Y Y Y Y Y Y Y Y Y Y Y Y Gn Cm Y Cm Mt, Pl Sl Cm, Fm, Sl Rb Mt Y Y Y Y Y Y Y Y Y Y Y Y Y Y Y Mt Rb Cm, Gl Cr, Mt Mt Mt Mt LS-DYNA Theory Manual Material Models Blatz-Ko Foam FLD Transversely Anisotropic 38 39 40 Nonlinear Orthotropic Y Y Fm, Pl Y Y Y Mt Y Y Cm 41- 50 42 User Defined Materials Y Y Y Y Y Y Y Y Gn Planar Anisotropic Plasticity Model Notes: Gn Gen- eral Cm Com- posites Cr Ce- ramics Fl Fluids Fm Foam Gl Glass Hy Hydro -dyn Mt Metal Pl Plastic Rb Rubber Sl Soil/C onc Material Title ff - - - ff 51 Bamman Plasticity) 52 Bamman Damage 53 Closed Cell Foam Polyurethane) (Temp/Rate Dependent Y Y Y Y Y Gn (Low Density Y Y Y Y Y Y Mt Fm Y 54 Composite Damage with Change Y Y Cm Failure 55 Composite Damage with Tsai-Wu Y Y Cm Failure 56 Low Density Urethane Foam 57 58 Laminated Composite Fabric 59 Composite Failure (Plasticity Based) Elastic with Viscosity (Viscous Glass) 60 61 Kelvin-Maxwell Viscoelastic 62 Viscous Foam (Crash Dummy Foam) 63 Isotropic Crushable Foam Y Y Y Fm Y Cm, Cr Y Y Y Y Y Y Y Y Y Y Y Y Y Gl Fm Fm Fm Material Models LS-DYNA Theory Manual (Rate/Temp 64 Rate Sensitive Powerlaw Plasticity 65 Zerilli-Armstrong Plasticity) Linear Elastic Discrete Beam 66 67 Nonlinear Elastic Discrete Beam 68 Nonlinear Plastic Discrete Beam 69 SID Damper Discrete Beam 70 Hydraulic Gas Damper Discrete Beam 71 Cable Discrete Beam (Elastic) 72 Concrete Damage Mt Y Y Y Y Y Y Y Y Y Mt Y Y Y Y Y Y Y Y Y Y Y Y Y Y Y Y Sl Notes: Gn General Cm Compo- sites Cr Ceramics Fluids Fl Fm Foam Gl Glass Hy Hydro- dyn Mt Metal Plastic Pl Rb Rubber Sl Soil/Con c Material Title ff - - - ff 73 Low Density Viscous Foam Y Y Y Fm 74 Elastic Spring for the Discrete Beam 75 Bilkhu/Dubois Foam (Isotropic) Y 76 General Viscoelastic (Maxwell Model) Y 77 Hyperelastic and Ogden Rubber 78 Soil Concrete Y Y Y Y Y 79 Hysteretic Soil (Elasto-Perfectly Y Y Fm Rb Rb Sl Sl Plastic) 80 Ramberg Osgood Plasticity 81 Plasticity with Damage (Elasto- Y Y Y Y Y Y Mt, Pl 82 Plastic) Isotropic Anisotropic Damage Elastic-Plastic with LS-DYNA Theory Manual Material Models 83 Fu Chang Foam 84 Winfrith Concrete Reinforcement Y Y Y Y Fm 85 86 Orthotropic Viscoelastic 87 Cellular Rubber 88 MTS 89 Plasticity Polymer 90 Acoustic 91 Soft Tissue Y Y Y Y Rb Rb Y Y Y Y Mt Y Y Y Y Fl 93 Elastic 6DOF Spring Discrete Beam Y 94 Inelastic Spring Discrete Beam Y Notes: Gn General Cm Compo- sites Cr Ceram- ics Fluids Fl Fm Foam Gl Glass Hy Hydro- dyn Mt Metal Plastic Pl Rb Rubber Sl Soil/Co nc ff - - - ff Material Title Inelastic 6DOF Spring Discrete Beam Y Brittle Damage Y Y Y 95 96 97 General Joint Discrete Beam Y 98 99 Simplified Johnson Cook Y Y Y Y Simplified Johnson Cook Orthotropic Damage 100 Spotweld LS-DYNA Draft Material Models LS-DYNA Theory Manual 101 GEPLASTIC Strate2000a 102 Inv Hyperbolic Sin 103 Anisotropic Viscoplastic 104 Damage 1 105 Damage 2 106 Elastic Viscoplastic Thermal Y Y Y Y Y Y Y Y Y Y Y 107 108 109 110 Johnson Holmquist Ceramics 111 Johnson Holmquist Concrete 112 Finite Elastic Strain Plasticity Y Y Y 113 TRIP Y Y Y Mt 114 Layered Linear Plasticity Y Y 115 Unified Creep Y Notes: Gn General Cm Compo- sites Cr Ceram- ics Fl Fluids Fm Foam Gl Glass Hy Hydro- dyn Mt Metal Plastic Pl Rb Rubber Sl Soil/Co nc Material Title 116 Composite Layup 117 Composite Matrix 118 Composite Direct ff - - - ff Y Y Y LS-DYNA Theory Manual Material Models 119 General Nonlinear 6DOF Discrete Y Y Y Beam 120 Gurson Y 121 Generalized Nonlinear 1DOF Discrete Y Beam 122 Hill 3RC 123 Modified Piecewise Linear Plasticity Y Y 124 Plasticity Compression Tension 126 Modified Honeycomb 127 Arruda Boyce Rubber 128 Heart Tissue 129 Lung Tissue Y Y Y Y Y 130 Special Orthotropic Y 131 Isotropic Smeared Crack 132 Orthotropic Smeared Crack 133 Barlat YLD2000 Y Y Y Mt, Cm Y Mt, Cm 139 Modified Force Limited Y 140 Vacuum 141 Rate Sensitive Polymer Notes: Gn General Cm Compo- sites Cr Ceramics Fl Fluids Fm Foam Gl Glass Hy Hydro- dyn Mt Metal Pl Plastic Rb Rubber Sl Soil/Con c Material Title ff - - - ff Material Models LS-DYNA Theory Manual 142 Transversely Anisotropic Crushable Foam 143 Wood 144 Pitzer Crushable Foam 145 Schwer Murray Cap Model 146 1DOF Generalized Spring 147 FHWA Soil 147 FHWA Soil Nebraska 148 Gas Mixture 150 CFD 151 EMMI 154 Deshpande Fleck Foam Y Y Y Y Y Mt 156 Muscle Y Y 158 Rate Sensitive Composite Fabric Y Y Y Y Cm 159 CSMC 161 Composite MSC 163 Modified Crushable Foam 164 Brain Linear Viscoelastic Y Y Y Sl Y Y 166 Moment Curvature Beam Y 169 Arup Adhesive 170 Resultant Anisotropic 175 Viscoelastic Thermal 176 Quasilinear Viscoelastic Y Y Y Y Y Pb Pl Y Y Y Y Y Rb LS-DYNA Theory Manual Material Models Notes: Gn General Cm Compo- sites Cr Ceramics Fl Fluids Fm Foam Gl Glass Hy Hydro- dyn Mt Metal Pl Plastic Rb Rubber Sl Soil/Con c ff - - - ff Material Title 177 Hill Foam 178 Viscoelastic Hill Foam 179 Low Density Synthetic Foam 181 Simplified Rubber 183 Simplified Rubber with Damage Y Y Y Y Y Rb 184 Cohesive Elastic 185 Cohesive TH 191 Seismic Beam 192 Soil Brick 193 Drucker Prager 194 RC Shear Wall 195 Concrete Beam 196 General Spring Discrete Beam 197 Seismic Isolator 198 Jointed Rock Spring Elastic (Linear) Y Y Y Y Y Y Y Y Y Y Y Y Cm, Mt Y Cm, Mt Y Mt Y Damper Viscous (Linear) Y Y Spring Elastoplastic (Isotropic) Y DS 1 DS 2 DS Material Models LS-DYNA Theory Manual Spring Nonlinear Elastic Y Y Damper Nonlinear Elastic Y Y Spring General Nonlinear Y DS 4 DS 5 DS 6 Material Title Spring Maxwell (Three Parameter Viscoelastic) Spring Compression) Spring Trilinear Degrading (Tension Inelastic or Spring Squat Shearwall Spring Muscle DS 7 DS 8 DS 13 DS 14 DS 15 SB1 Seatbelt Notes: Gn General Cm Compo- sites Cr Ceramics Fl Fluids Fm Foam Gl Glass Hy Hydro- dyn Mt Metal Pl Plastic Rb Rubber Sl Soil/Con c ff - - - ff Y Y Y T01 Thermal Isotropic T02 Thermal Orthotropic Y Y Y Y T03 Thermal Isotropic (Temp. Y Y Dependent) T04 Thermal Orthotropic (Temp. Y Y Dependent) T05 Thermal Isotropic (Phase Change) Y Y Y Y Y Y Y LS-DYNA Theory Manual Material Models T06 Thermal Isotropic (Temp Dep-Load Y Y Curve) T11 Thermal User Defined Y Y Y Y Material Models LS-DYNA Theory Manual 22.1 Material Model 1: Elastic In this elastic material we compute the co-rotational rate of the deviatoric Cauchy stress tensor as and pressure ∇𝑛+1 2⁄ 𝑠𝑖𝑗 = 2𝐺𝜀̇𝑖𝑗 ′ 𝑛+1 2⁄ , 𝑝𝑛+1 = −𝐾ln𝑉𝑛+1, (22.1.1) (22.1.2) where 𝐺 and 𝐾 are the elastic shear and bulk moduli, respectively, and 𝑉 is the relative volume, i.e., the ratio of the current volume to the initial volume. LS-DYNA Theory Manual Material Models 22.2 Material Model 2: Orthotropic Elastic The material law that relates second Piola-Kirchhoff stress 𝐒 to the Green-St. Venant strain 𝐄 is 𝐒 = 𝐂 ⋅ 𝐄 = 𝐓T𝐂l𝐓 ⋅ 𝐄, where 𝐓 is the transformation matrix [Cook 1974]. 𝐓 = 𝑙1 ⎡ ⎢ 𝑙2 ⎢ ⎢ 𝑙3 ⎢ ⎢ 2𝑙1𝑙2 ⎢ 2𝑙2𝑙3 ⎢ 2𝑙3𝑙1 ⎣ 𝑚1 𝑚2 𝑚3 2𝑚1𝑚2 2𝑚2𝑚3 2𝑚3𝑚1 𝑛1 𝑛2 𝑛3 2𝑛1𝑛2 2𝑛2𝑛3 2𝑛3𝑛1 𝑙1𝑚1 𝑙2𝑚2 𝑙3𝑚3 (𝑙1𝑚2 + 𝑙1𝑚1) (𝑙2𝑚3 + 𝑙3𝑚2) (𝑙3𝑚1 + 𝑙1𝑚3) 𝑚1𝑛1 𝑚2𝑛2 𝑚3𝑛3 (𝑚1𝑛2 + 𝑚2𝑛1) (𝑚2𝑛3 + 𝑚3𝑛2) (𝑚3𝑛1 + 𝑚1𝑛3) 𝑛1𝑙1 ⎤ ⎥ 𝑛2𝑙2 ⎥ ⎥ 𝑛3𝑙3 ⎥ ⎥ (𝑛1𝑙2 + 𝑛2𝑙1) ⎥ (𝑛2𝑙3 + 𝑛3𝑙2) ⎥ (𝑛3𝑙1 + 𝑛1𝑙3)⎦ , 𝑙𝑖, 𝑚𝑖, 𝑛𝑖 are the direction cosines (22.2.1) (22.2.2) (22.2.3) ′ denotes the material axes. The constitutive matrix 𝐂l is defined in terms of the ′ = 𝑙𝑖𝑥1 + 𝑚𝑖𝑥2 + 𝑛𝑖𝑥3, 𝑥𝑖 𝑖 = 1, 2, 3, and 𝑥𝑖 material axes as −1 = 𝐂l 𝐸11 𝜐12 𝐸11 𝜐13 𝐸11 − − 𝜐21 𝐸22 𝐸22 𝜐23 𝐸22 − − 𝜐31 𝐸33 𝜐32 𝐸33 𝐸33 𝐺12 𝐺23 ⎤ ⎥ ⎥ ⎥ ⎥ ⎥ ⎥ ⎥ ⎥ , ⎥ ⎥ ⎥ ⎥ ⎥ ⎥ ⎥ ⎥ 𝐺31⎦ − − ⎡ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎣ where the subscripts denote the material axes, i.e., 𝜐𝑖𝑗 = 𝜐𝑥𝑖 ′ ′𝑥𝑗 and ′. 𝐸𝑖𝑖 = 𝐸𝑥𝑖 Since 𝐂l is symmetric 𝜐12 𝐸11 = 𝜐21 𝐸22 , etc. The vector of Green-St. Venant strain components is 𝐄T = [𝐸11 𝐸22 𝐸33 𝐸12 𝐸23 𝐸31]. (22.2.4) (22.2.5) (22.2.6) (22.2.7) Material Models LS-DYNA Theory Manual After computing 𝑆𝑖𝑗, we use Equation (21.32) to obtain the Cauchy stress. This model will predict realistic behavior for finite displacement and rotations as long as the strains are small. LS-DYNA Theory Manual Material Models 22.3 Material Model 3: Elastic Plastic with Kinematic Hardening Isotropic, kinematic, or a combination of isotropic and kinematic hardening may be obtained by varying a parameter, called 𝛽 between 0 and 1. For 𝛽 equal to 0 and 1, respectively, kinematic and isotropic hardening are obtained as shown in Figure 22.3.1. Krieg and Key [1976] formulated this model and the implementation is based on their paper. In isotropic hardening, the center of the yield surface is fixed but the radius is a function of the plastic strain. In kinematic hardening, the radius of the yield surface is fixed but the center translates in the direction of the plastic strain. Thus the yield condition is where 𝜙 = 𝜉𝑖𝑗𝜉𝑖𝑗 − 𝜎𝑦 = 0, 𝜉𝑖𝑗 = 𝑠𝑖𝑗 − 𝛼𝑖𝑗 p . 𝜎𝑦 = 𝜎0 + 𝛽𝐸p𝜀eff The co-rotational rate of 𝛼𝑖𝑗 is ∇ = (1 − 𝛽) 𝛼𝑖𝑗 p. 𝐸p𝜀̇𝑖𝑗 Hence, 𝑛+1 = 𝛼𝑖𝑗 𝛼𝑖𝑗 𝑛 + (𝛼𝑖𝑗 ∇𝑛+1 2⁄ 𝑛+1 2⁄ + 𝛼𝑖𝑘 𝑛 𝛺𝑘𝑗 𝑛+1 2⁄ + 𝛼𝑗𝑘 𝑛 𝛺𝑘𝑖 (22.3.1) (22.3.2) (22.3.3) (22.3.4) (22.3.5) ) Δ𝑡𝑛+1 2⁄ . Strain rate is accounted for using the Cowper-Symonds [Jones 1983] model which scales the yield stress by a strain rate dependent factor ⎤ ⎥ ⎦ where 𝑝 and 𝐶 are user defined input constants and 𝜀̇ is the strain rate defined as: (𝜎0 + 𝛽𝐸p𝜀eff 𝜎𝑦 = 1 + ( p ), ⎡ ⎢ ⎣ ) 𝜀̇ 𝜀̇ = √𝜀̇𝑖𝑗𝜀̇𝑖𝑗. (22.3.6) (22.3.7) Material Models LS-DYNA Theory Manual δx Yield Stress ⎛ ⎜ ⎝ ⎛ ⎜ ⎝ l0 ln β=0, kinematic hardening β=1, isotropic hardening Figure 22.3.1. Elastic-plastic behavior with isotropic and kinematic hardening where l0 and l are the undeformed and deformed length of uniaxial tension specimen, respectively. The current radius of the yield surface, 𝜎𝑦, is the sum of the initial yield strength, p , where 𝐸p is the plastic hardening modulus 𝜎0, plus the growth 𝛽𝐸p𝜀eff and 𝜀eff p is the effective plastic strain 𝐸p = 𝐸t𝐸 𝐸 − 𝐸t , p = ∫ ( 𝜀eff 2⁄ p) p𝜀̇𝑖𝑗 𝜀̇𝑖𝑗 𝑑𝑡 . (22.3.8) (22.3.9) The plastic strain rate is the difference between the total and elastic (right superscript e) strain rates: p = 𝜀̇𝑖𝑗 − 𝜀̇𝑖𝑗 e . 𝜀̇𝑖𝑗 (22.3.10) In the implementation of this material model, the deviatoric stresses are updated elastically, as described for model 1, but repeated here for the sake of clarity: ∗ = 𝜎𝑖𝑗 𝜎𝑖𝑗 𝑛 + 𝐶𝑖𝑗𝑘𝑙Δ𝜀𝑘𝑙, (22.3.11) where ∗ 𝜎𝑖𝑗 𝑛 𝜎𝑖𝑗 C𝑖𝑗𝑘𝑙 is the trial stress tensor, is the stress tensor from the previous time step, is the elastic tangent modulus matrix, LS-DYNA Theory Manual Material Models Δ𝜀𝑘𝑙 is the incremental strain tensor. and, if the yield function is satisfied, nothing else is done. If, however, the yield function is violated, an increment in plastic strain is computed, the stresses are scaled back to the yield surface, and the yield surface center is updated. Let s𝑖𝑗 ∗ represent the trial elastic deviatoric stress state at 𝑛 + 1 and ∗ = σ𝑖𝑗 s𝑖𝑗 ∗ − ∗ , σ𝑘𝑘 ∗ = s𝑖𝑗 ξ𝑖𝑗 ∗ − α𝑖𝑗. Define the yield function, (22.3.12) (22.3.13) 𝜙 = ∗𝜉𝑖𝑗 𝜉𝑖𝑗 ∗ − 𝜎𝑦 2 = 𝛬2 − 𝜎𝑦 2 { ≤ 0 > 0 for elastic or neutral loading for plastic harding , (22.3.14) For plastic hardening then p𝑛+1 𝜀eff p𝑛 = 𝜀eff + 𝛬 − 𝜎𝑦 3𝐺 + 𝐸p p𝑛 = 𝜀eff p , + Δ𝜀eff scale back the stress deviators and update the center: 𝑛+1 = 𝜎𝑖𝑗 𝜎𝑖𝑗 ∗ − 3𝐺Δ𝜀eff ∗, 𝜉𝑖𝑗 𝑛 + 1 = 𝛼𝑖𝑗 𝛼𝑖𝑗 𝑛 + (1 − 𝛽)𝐸pΔ𝜀eff ∗. 𝜉𝑖𝑗 (22.3.15) (22.3.16) (22.3.17) Plane Stress Plasticity The plane stress plasticity options apply to beams, shells, and thick shells. Since the stresses and strain increments are transformed to the lamina coordinate system for the constitutive evaluation, the stress and strain tensors are in the local coordinate system. The application of the Jaumann rate to update the stress tensor allows for the possibility that the normal stress, 𝜎33, will not be zero. The first step in updating the stress tensor is to compute a trial plane stress update assuming that the incremental strains are elastic. In the above, the normal strain increment Δ𝜀33 is replaced by the elastic strain increment Δ𝜀33 = − 𝜎33 + 𝜆(Δ𝜀11 + Δ𝜀22) 𝜆 + 2𝜇 , (22.3.18) where 𝜆 and 𝜇 are Lamé’s constants. Material Models LS-DYNA Theory Manual When the trial stress is within the yield surface, the strain increment is elastic and the stress update is completed. Otherwise, for the plastic plane stress case, secant iteration is used to solve Equation (22.3.16) for the normal strain increment (Δ𝜀33) required to produce a zero normal stress: 𝑖 = 𝜎33 𝜎33 ∗ − p𝑖 3𝐺Δ𝜀eff 𝜉33 , (22.3.19) Here, the superscript 𝑖 indicates the iteration number. The secant iteration formula for Δε33 (the superscript p is dropped for clarity) is 𝑖−1 𝑖 − Δ𝜀33 Δ𝜀33 𝑖−1 𝜎33 𝑖 − 𝜎33 𝜎33 where the two starting values are obtained from the initial elastic estimate and by assuming a purely plastic increment, i.e., 𝑖+1 = Δ𝜀33 𝑖−1 − (22.3.20) Δ𝜀33 𝑖−1, 1 = −(Δ𝜀11 − Δ𝜀22). These starting values should bound the actual values of the normal strain increment. Δ𝜀33 (22.3.21) The iteration procedure uses the updated normal stain increment to update first the deviatoric stress and then the other quantities needed to compute the next estimate of the normal stress in Equation (22.3.19). The iterations proceed until the normal stress is sufficiently small. The convergence criterion requires convergence of the normal 𝜎33 strains: ∣Δ𝜀33 𝑖 − Δ𝜀33 𝑖−1∣ 𝑖+1∣ ∣Δ𝜀33 < 10−4. (22.3.22) After convergence, the stress update is completed using the relationships given in Equations (22.3.16) and (22.3.17) LS-DYNA Theory Manual Material Models 22.4 Material Model 4: Thermo-Elastic-Plastic This model was adapted from the NIKE2D [Hallquist 1979] code. A more complete description of its formulation is given in the NIKE2D user’s manual. Letting 𝑇 represent the temperature, we compute the elastic co-rotational stress rate as where ∇ = 𝐶𝑖𝑗𝑘𝑙(𝜀̇𝑘𝑙 − ε̇𝑘𝑙 𝜎𝑖𝑗 T ) + 𝜃̇ 𝑖𝑗𝑑𝑇, 𝜃̇ 𝑖𝑗 = 𝑑𝐶𝑖𝑗𝑘𝑙 𝑑𝑇 −1 𝜎̇𝑚𝑛, 𝐶𝑘𝑙𝑚𝑛 and 𝐶𝑖𝑗𝑘𝑙 is the temperature dependent elastic constitutive matrix: 𝐶𝑖𝑗𝑘𝑙 = (1 + 𝜐)(1 − 2𝜐) ⎡1 − 𝜐 ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎣ 1 − 𝜐 1 − 𝜐 1 − 2𝜐 1 − 2𝜐 1 − 2𝜐 ⎤ ⎥ ⎥ ⎥ ⎥ ⎥ ⎥ ⎥ , ⎥ ⎥ ⎥ ⎥ ⎥ ⎥ ⎥ ⎥ ⎦ (22.4.1) (22.4.2) (22.4.3) where 𝜐 is Poisson’s ratio. The thermal strain rate can be written in terms of the coefficient of thermal expansion 𝛼 as: T = 𝛼𝑇̇𝛿𝑖𝑗, 𝜀̇𝑖𝑗 (22.4.4) When treating plasticity, we use a procedure analogous to that for material 3. We update the stresses elastically and check to see if we violate the isotropic yield function where 𝜙 = 𝑠𝑖𝑗𝑠𝑖𝑗 − 𝜎𝑦(𝑇)2 , p . 𝜎𝑦(𝑇) = 𝜎𝑜(𝑇) + 𝐸p(𝑇)𝜀eff (22.4.5) (22.4.6) Material Models LS-DYNA Theory Manual The initial yield, 𝜎o, and plastic hardening modulus, 𝐸p, are temperature dependent. If the behavior is elastic we do nothing; otherwise, we scale back the stress deviators by the factor 𝑓s: where 𝑛+1 = 𝑓s𝑠𝑖𝑗 ∗ , 𝑠𝑖𝑗 𝑓s = 𝜎𝑦 2⁄ ∗ ) ∗ 𝑠𝑖𝑗 𝑠𝑖𝑗 (3 , and update the plastic strain by the increment p = Δ𝜀eff 2⁄ (1 − 𝑓s)(3 ∗ ) ∗ 𝑠𝑖𝑗 𝑠𝑖𝑗 𝐺 + 3𝐸p . (22.4.7) (22.4.8) (22.4.9) LS-DYNA Theory Manual Material Models 22.5 Material Model 5: Soil and Crushable Foam This model, due to Krieg [1972], provides a simple model for foam and soils whose material properties are not well characterized. We believe the other foam models in LS-DYNA are superior in their performance and are recommended over this model which simulates the crushing through the volumetric deformations. If the yield stress is too low, this foam model gives nearly fluid like behavior. A pressure-dependent flow rule governs the deviatoric behavior: 𝜙s = s𝑖𝑗s𝑖𝑗 − (𝑎0 + 𝑎1𝑝 + 𝑎2𝑝2), (22.5.1) where 𝑎0, 𝑎1, and 𝑎2 are user-defined constants. Volumetric yielding is determined by a tabulated curve of pressure versus volumetric strain. Elastic unloading from this curve is assumed to a tensile cutoff as illustrated in Figure 22.5.1. Implementation of this model is straightforward. One history variable, the maximum volumetric strain in compression, is stored. If the new compressive volumetric strain exceeds the stored value, loading is indicated. When the yield ∗ , are scaled back using a simple radial condition is violated, the updated trial stresses, 𝑠𝑖𝑗 Loading and unloading (along the grey arows) follows the input curve when the volumetric crushing option is off (VCR = 1.0) tension compression Volumetric Strain, ln ⎛ ⎜ ⎝ ⎛ ⎜ V0 ⎝ Pressure Cutoff Value The bulk unloading modulus is used if the volumetric crushing option is on (VCR = 0). In thiscase the aterial's response follows the black arrows. Figure 22.5.1. Volumetric strain versus pressure curve for soil and crushable foam model. return algorithm: Material Models LS-DYNA Theory Manual 𝑛+1 = s𝑖𝑗 ⎜⎜⎜⎛𝑎0 + 𝑎1𝑝 + a2𝑝2 s𝑖𝑗s𝑖𝑗 ⎝ 2⁄ ⎟⎟⎟⎞ ⎠ ∗ . s𝑖𝑗 (22.5.2) If the hydrostatic tension exceeds the cutoff value, the pressure is set to the cutoff value and the deviatoric stress tensor is zeroed. LS-DYNA Theory Manual Material Models 22.6 Material Model 6: Viscoelastic In this model, linear viscoelasticity is assumed for the deviatoric stress tensor [Herrmann and Peterson 1968]: where 𝑠𝑖𝑗 = 2 ∫ 𝜙(𝑡 − 𝜏) ′ (𝜏) ∂𝜀𝑖𝑗 ∂𝜏 𝑑𝜏 , 𝜙(𝑡) = G∞ + (G0 − G∞)𝑒−𝛽𝑡, (22.6.1) (22.6.2) is the shear relaxation modulus. A recursion formula is used to compute the new value of the hereditary integral at time 𝑡𝑛+1 from its value at time 𝑡𝑛. Elastic bulk behavior is assumed: 𝑝 = 𝐾ln𝑉, (22.6.3) where pressure is integrated incrementally. Material Models LS-DYNA Theory Manual 22.7 Material Model 7: Continuum Rubber The hyperelastic continuum rubber model was studied by Blatz and Ko [1962]. In this model, the second Piola-Kirchhoff stress is given by 𝑆𝑖𝑗 = 𝐺 (𝑉 −1𝐶𝑖𝑗 − 𝑉 − 1 1−2𝜐𝛿𝑖𝑗), (22.7.1) where 𝐺 is the shear modulus, 𝑉 is the relative volume, 𝜐 is Poisson’s ratio, and 𝐶𝑖𝑗 is the right Cauchy-Green strain: C𝑖𝑗 = 𝜕𝑥𝑘 𝜕𝑋𝑖 𝜕𝑥𝑘 𝜕𝑋𝑗 , (22.7.2) after determining 𝑆𝑖𝑗, it is transformed into the Cauchy stress tensor, 𝜎𝑖𝑗: 𝜕𝑥𝑗 𝜕𝑋𝑙 where 𝜌0 and 𝜌 are the initial and current density, respectively. The default value of υ is 0.463. 𝜕𝑥𝑖 𝜕𝑋𝑘 𝜎𝑖𝑗 = 𝜌0 (22.7.3) 𝑆𝑘𝑙, LS-DYNA Theory Manual Material Models 22.8 Material Model 8: Explosive Burn Burn fractions, which multiply the equations of states for high explosives, control the release of chemical energy for simulating detonations. In the initialization phase, a lighting time 𝑡1 is computed for each element by dividing the distance from the detonation point to the center of the element by the detonation velocity 𝐷. If multiple detonation points are defined, the closest point determines 𝑡1. The burn fraction 𝐹 is taken as the maximum 𝐹 = max(𝐹1, 𝐹2), (22.8.1) where 𝐹1 = ) 3 ( 𝑣e 𝐴emax ⎧ 2 (𝑡 − 𝑡𝑙)𝐷 { { {{ { ⎨ {{ { {{ ⎩ 0 𝐹2 = 1 − 𝑉 1 − 𝑉CJ , 𝑡 > 𝑡l 𝑡 ≤ 𝑡l (22.8.2) (22.8.3) where 𝑉CJ is the Chapman-Jouguet relative volume and 𝑡 is current time. If 𝐹 exceeds 1, it is reset to 1. This calculation of the burn fraction usually requires several time steps for 𝐹 to reach unity, thereby spreading the burn front over several elements. After reaching unity, 𝐹 is held constant. This burn fraction calculation is based on work by Wilkins [1964] and is also discussed by Giroux [1973]. As an option, the high explosive material can behave as an elastic perfectly- plastic solid prior to detonation. In this case we update the stress tensor, to an elastic trial stress, 𝑠𝑖𝑗 ∗𝑛+1, ∗𝑛+1 = 𝑠𝑖𝑗 𝑠𝑖𝑗 𝑛 + 𝑠𝑖𝑝𝛺𝑝𝑗 + 𝑠𝑗𝑝𝛺𝑝𝑖 + 2𝐺𝜀̇𝑖𝑗 ′ 𝑑𝑡, (22.8.4) where 𝐺 is the shear modulus, and 𝜀̇𝑖𝑗 condition is given by: ′ is the deviatoric strain rate. The von Mises yield 𝜎𝑦 where the second stress invariant, 𝐽2, is defined in terms of the deviatoric stress components as 𝜙 = 𝐽2 − (22.8.5) , 𝐽2 = 𝑠𝑖𝑗𝑠𝑖𝑗, (22.8.6) Material Models LS-DYNA Theory Manual and the yield stress is 𝜎𝑦. If yielding has occurred, i.e., 𝜙 > 0, the deviatoric trial stress is scaled to obtain the final deviatoric stress at time 𝑛 + 1: If 𝜙 ≤ 0, then 𝑛+1 = 𝑠𝑖𝑗 𝜎𝑦 √3𝐽2 ∗𝑛+1, 𝑠𝑖𝑗 𝑛+1 = 𝑠𝑖𝑗 𝑠𝑖𝑗 ∗𝑛+1. Before detonation pressure is given by the expression 𝑝𝑛+1 = 𝐾 ( 𝑉𝑛+1 − 1). where K is the bulk modulus. Once the explosive material detonates: and the material behaves like a gas. 𝑛+1 = 0. 𝑠𝑖𝑗 (22.8.7) (22.8.8) (22.8.9) (22.8.10) The shadow burn option should be active when computing the lighting time if there exist elements within the mesh for which there is no direct line of sight from the detonation points. The shadow burn option is activated in the control section. The lighting time is based on the shortest distance through the explosive material. If inert obstacles exist within the explosive material, the lighting time will account for the extra time required for the detonation wave to travel around the obstacles. The lighting times also automatically accounts for variations in the detonation velocity if different explosives are used. No additional input is required for the shadow option but care must be taken when setting up the input. This option works for two and three- dimensional solid elements. It is recommended that for best results: 1. Keep the explosive mesh as uniform as possible with elements of roughly the same dimensions. 2. 3. Inert obstacle such as wave shapers within the explosive must be somewhat larger than the characteristic element dimension for the automatic tracking to function properly. Generally, a factor of two should suffice. The characteristic element dimension is found by checking all explosive elements for the largest diagonal The detonation points should be either within or on the boundary of the explosive. Offset points may fail to initiate the explosive. 4. Check the computed lighting times in the post processor LS-PrePost. The lighting times may be displayed at time = 0, state 1, by plotting component 7 (a component normally reserved for plastic strain) for the explosive material. The lighting times are stored as negative numbers. The negative lighting time is replaced by the burn fraction when the element ignites. LS-DYNA Theory Manual Material Models 5. Line detonations may be approximated by using a sufficient number of detonation points to define the line. Too many detonation points may result in significant initialization cost. Material Models LS-DYNA Theory Manual 22.9 Material Model 9: Null Material For solid elements equations of state can be called through this model to avoid deviatoric stress calculations. A pressure cutoff may be specified to set a lower bound on the pressure. This model has been very useful when combined with the reactive high explosive model where material strength is often neglected. The null material should not be used to delete solid elements. An optional viscous stress of the form ′ , 𝜎𝑖𝑗 = 𝜇𝜀̇𝑖𝑗 ′ is the deviatoric strain rate. is computed for nonzero 𝜇 where 𝜀̇𝑖𝑗 (22.9.1) Sometimes it is advantageous to model contact surfaces via shell elements which are not part of the structure, but are necessary to define areas of contact within nodal rigid bodies or between nodal rigid bodies. Beams and shells that use this material type are completely bypassed in the element processing. The Young’s modulus and Poisson’s ratio are used only for setting the contact interface stiffnesses, and it is recommended that reasonable values be input. LS-DYNA Theory Manual Material Models 22.10 Material Model 10: Elastic-Plastic-Hydrodynamic For completeness we give the entire derivation of this constitutive model based on radial return plasticity. The pressure, 𝑝, deviatoric strain rate, 𝜀̇𝑖𝑗 strain rate, and 𝜀̇v, are defined in Equation (1.1.1): ′ , deviatoric stress rate, 𝑠 ̇𝑖𝑗, volumetric 𝜎𝑖𝑗𝛿𝑖𝑗 𝑝 = − 𝑠𝑖𝑗 = 𝜎𝑖𝑗 + 𝑝𝛿𝑖𝑗 ∇ = 2𝜇𝜀̇𝑖𝑗 𝑠𝑖𝑗 ′ = 𝜀̇𝑖𝑗 − 𝜀̇𝑖𝑗 𝜀̇v = 𝜀̇𝑖𝑗𝛿𝑖𝑗 ′ . ′ = 2𝐺𝜀̇𝑖𝑗 𝜀̇v The Jaumann rate of the deviatoric stress, 𝑠𝑖𝑗 ∇, is given by: ∇ = 𝑠 ̇𝑖𝑗 − 𝑠𝑖𝑝𝛺𝑝𝑗 − 𝑠𝑗𝑝𝛺𝑝𝑖. 𝑠𝑖𝑗 First we update s𝑖𝑗 𝑛+1 = 𝑠𝑖𝑗 𝑖𝑗 ∗ 𝑠 𝑛 to s𝑖𝑗 𝑛+1 elastically 𝑛 + 𝑠𝑖𝑝𝛺𝑝𝑗 + 𝑠𝑗𝑝𝛺𝑝𝑖 + 2𝐺𝜀̇𝑖𝑗 ′ 𝑑𝑡 = 𝑠𝑖𝑗 𝑛 + 𝑅𝑖𝑗⏟ 𝑅𝑛 𝑠𝑖𝑗 (22.10.1) (22.10.2) (22.10.3) ′ 𝑑𝑡⏟ + 2𝐺𝜀̇𝑖𝑗 ′ 2𝐺Δ𝜀𝑖𝑗 , where the left superscript, *, denotes a trial stress value. The effective trial stress is defined by 𝑠∗ = ( 𝑠∗ 𝑛+1 𝑠∗ 𝑖𝑗 𝑛+1) 𝑖𝑗 2⁄ , and if 𝑠∗ exceeds yield stress 𝜎y, the Von Mises flow rule: 𝜙 = 𝑠𝑖𝑗𝑠𝑖𝑗 − 𝜎y ≤ 0, (22.10.4) (22.10.5) is violated and we scale the trial stresses back to the yield surface, i.e., a radial return 𝑛+1 = 𝑠𝑖𝑗 𝜎𝑦 𝑠∗ 𝑠∗ 𝑛+1 = 𝑚 𝑠∗ 𝑖𝑗 𝑛+1. 𝑖𝑗 (22.10.6) The plastic strain increment can be found by subtracting the deviatoric part of R𝑛 𝑛+1 − 𝑠𝑖𝑗 ), from the total deviatoric increment, the strain increment that is elastic, 1 Δε𝑖𝑗 ′ , i.e., 2𝐺 (𝑠𝑖𝑗 p = Δ𝜀𝑖𝑗 ′ − Δ𝜀𝑖𝑗 2𝐺 R𝑛 𝑛+1 − 𝑠𝑖𝑗 (𝑠𝑖𝑗 ). (22.10.7) Material Models LS-DYNA Theory Manual Recalling that, ′ = Δ𝜀𝑖𝑗 ∗ ( 𝑠 R𝑛 𝑛+1 − 𝑠𝑖𝑗 𝑖𝑗 2𝐺 ) , and substituting Equation (22.10.8) into (22.10.7) we obtain, p = Δ𝜀𝑖𝑗 ∗ ( 𝑠 𝑛+1 − 𝑠𝑖𝑗 𝑖𝑗 2𝐺 𝑛+1) . Substituting Equation (22.10.6) 𝑛+1 = 𝑚 𝑠∗ 𝑠𝑖𝑗 𝑛+1, 𝑖𝑗 into Equation (22.10.9) gives, p = ( Δ𝜀𝑖𝑗 1 − 𝑚 2𝐺 ) 𝑠∗ 𝑛+1 = 𝑖𝑗 1 − 𝑚 2𝐺𝑚 𝑛+1 = 𝑑λ𝑠𝑖𝑗 𝑠𝑖𝑗 𝑛+1. By definition an increment in effective plastic strain is Δ𝜀p = ( 2⁄ p) pΔ𝜀𝑖𝑗 Δ𝜀𝑖𝑗 . Squaring both sides of Equation (22.10.11) leads to: Δ𝜀𝑖𝑗 pΔ𝜀𝑖𝑗 p = ( 1 − 𝑚 2𝐺 ) 𝑠∗ 𝑛+1 𝑠∗ 𝑖𝑗 𝑛+1 𝑖𝑗 or from Equations (22.10.4) and (22.10.12): Hence, Δ𝜀p2 = ( 1 − 𝑚 2𝐺 2 2 ) 𝑠∗2 Δ𝜀p = 1 − 𝑚 3𝐺 𝑠∗ = 𝑠∗ − 𝜎y 3𝐺 where we have substituted for m from Equation (22.10.6) 𝑚 = 𝜎y 𝑠∗ If isotropic hardening is assumed then: 𝑛+1 = 𝜎y 𝜎y 𝑛 + 𝐸pΔ𝜀p and from Equation (22.10.15) Δ𝜀p = 𝑛+1) (𝑠∗ − 𝜎y 3𝐺 = (𝑠∗ − 𝜎y 𝑛 − 𝐸pΔ𝜀p) . 3𝐺 Thus, (22.10.8) (22.10.9) (22.10.10) (22.10.11) (22.10.12) (22.10.13) (22.10.14) (22.10.15) (22.10.16) (22.10.17) (22.10.18) LS-DYNA Theory Manual Material Models and solving for the incremental plastic strain gives (3𝐺 + 𝐸p)Δ𝜀p = (𝑠∗ − 𝜎y 𝑛), Δ𝜀p = 𝑛) (𝑠∗ − 𝜎y . (3𝐺 + 𝐸p) (22.10.19) (22.10.20) The algorithm for plastic loading can now be outlined in five simple stress. If the effective trial stress exceeds the yield stress then 1. Solve for the plastic strain increment: 𝑛) (𝑠∗ − σy . (3𝐺 + 𝐸p) Δ𝜀p = 2. Update the plastic strain: 𝜀p𝑛+1 = 𝜀p𝑛 + Δ𝜀p. 3. Update the yield stress: 𝑛+1 = 𝜎y 𝜎y 𝑛 + 𝐸pΔ𝜀p. 4. Compute the scale factor using the yield strength at time 𝑛 + 1: 𝑚 = 𝑛+1 𝜎y 𝑠∗ . 5. Radial return the deviatoric stresses to the yield surface: 𝑛+1 = 𝑚 𝑠∗ 𝑠𝑖𝑗 𝑛+1. 𝑖𝑗 (22.10.21) (22.10.22) (22.10.23) (22.10.24) (22.10.25) Material Models LS-DYNA Theory Manual 22.11 Material Model 11: Elastic-Plastic With Thermal Softening Steinberg and Guinan [1978] developed this model for treating plasticity at high strain rates (105 s-1) where enhancement of the yield strength due to strain rate effects is saturated out. Both the shear modulus 𝐺 and yield strength 𝜎y increase with pressure but decrease with temperature. As a melt temperature is reached, these quantities approach zero. We define the shear modulus before the material melts as 𝐺 = 𝐺0 [1 + 𝑏𝑝𝑉 3⁄ − ℎ ( 𝐸 − 𝐸c 3𝑅′ − 300)] 𝑒 − 𝑓𝐸 𝐸m−𝐸, where 𝐺0, 𝑏, ℎ, and 𝑓 are input parameters, 𝐸c is the cold compression energy: 𝐸c(𝑋) = ∫ 𝑝𝑑𝑥 − 900𝑅′exp(𝑎𝑥) 2(𝛾𝑜−𝑎−1 ) (1 − 𝑋) , where, 𝑋 = 1 − 𝑉, and 𝐸m is the melting energy: 𝐸m(𝑋) = 𝐸c(𝑋) + 3𝑅′𝑇m(𝑋), which is a function of the melting temperature 𝑇m(𝑋): 𝑇m(𝑋) = 𝑇moexp(2𝑎𝑋) 2(𝛾𝑜−𝑎−1 ) (1 − 𝑋) , (22.11.1) (22.11.2) (22.11.3) (22.11.4) (22.11.5) and the melting temperature 𝑇mo at 𝜌 = 𝜌0. The constants 𝛾0 and a are input parameters. In the above equation, 𝑅′ is defined by 𝑅′ = 𝑅𝜌0 , (22.11.6) where 𝑅 is the gas constant and A is the atomic weight. The yield strength 𝜎y is given by: 𝜎y = 𝜎0 ′ [1 + 𝑏′𝑝𝑉 3 − ℎ ( 𝐸 − 𝐸c 3𝑅′ − 300)] 𝑒 − 𝑓𝐸 𝐸m−𝐸. If 𝐸m exceeds 𝐸𝑖. Here, 𝜎0 ′ is given by: ′ = 𝜎0[1 + 𝛽(𝛾𝑖 + 𝜀̅𝑝)]𝑛. 𝜎0 (22.11.7) (22.11.8) LS-DYNA Theory Manual Material Models where 𝛾1 is the initial plastic strain, and 𝑏′ and 𝜎0 exceeds 𝜎max, the maximum permitted yield strength, 𝜎0 the material melts, 𝜎y and 𝐺 are set to zero. ′ ′ are input parameters. Where 𝜎0 ′ is set to equal to 𝜎max. After LS-DYNA fits the cold compression energy to a ten-term polynomial expansion: 𝜂𝑖, (22.11.9) 𝐸c = ∑ 𝐸𝐶𝑖 𝑖=0 𝜌0 where 𝐸𝐶𝑖 is the ith coefficient and 𝜂 = the fit [Kreyszig 1972]. The ten coefficients may also be specified in the input. . The least squares method is used to perform Once the yield strength and shear modulus are known, the numerical treatment is similar to that for material model 10. Material Models LS-DYNA Theory Manual 22.12 Material Model 12: Isotropic Elastic-Plastic The von Mises yield condition is given by: 𝜎y where the second stress invariant, 𝐽2, is defined in terms of the deviatoric stress components as 𝜙 = 𝐽2 − (22.12.1) , 𝐽2 = 𝑠𝑖𝑗𝑠𝑖𝑗, (22.12.2) and the yield stress, 𝜎y, is a function of the effective plastic strain, 𝜀eff hardening modulus, 𝐸p: p , and the plastic p . 𝜎y = 𝜎0 + 𝐸p𝜀eff (22.12.3) The effective plastic strain is defined as p = ∫ 𝑑𝜀eff 𝜀eff , (22.12.4) p = √2 where 𝑑𝜀eff input tangent modulus, 𝐸t, as 3 𝑑𝜀𝑖𝑗 p𝑑𝜀𝑖𝑗 p, and the plastic tangent modulus is defined in terms of the 𝐸p = 𝐸𝐸t 𝐸 − 𝐸t . (22.12.5) Pressure is given by the expression 𝑉𝑛+1 − 1), where 𝐾 is the bulk modulus. This is perhaps the most cost effective plasticity model. Only one history variable, 𝜀eff p , is stored with this model. 𝑝𝑛+1 = 𝐾 ( (22.12.6) This model is not recommended for shell elements. In the plane stress implementation, a one-step radial return approach is used to scale the Cauchy stress tensor to if the state of stress exceeds the yield surface. This approach to plasticity leads to inaccurate shell thickness updates and stresses after yielding. This is the only model in LS-DYNA for plane stress that does not default to an iterative approach. LS-DYNA Theory Manual Material Models 22.13 Material Model 13: Isotropic Elastic-Plastic with Failure This highly simplistic failure model is occasionally useful. Material model 12 is called to update the stress tensor. Failure is initially assumed to occur if either 𝑝𝑛+1 < 𝑝min, (22.13.1) or p > 𝜀max 𝜀eff , (22.13.2) where 𝑝min and 𝜀max may never be negative and the deviatoric components are set to zero: are user-defined parameters. Once failure has occurred, pressure for all time. The failed element can only carry loads in compression. 𝑠𝑖𝑗 = 0 (22.13.3) Material Models LS-DYNA Theory Manual 22.14 Material Model 14: Soil and Crushable Foam With Failure This material model provides the same stress update as model 5. However, if pressure ever reaches its cutoff value, failure occurs and pressure can never again go negative. In material model 5, the pressure is limited to its cutoff value in tension. LS-DYNA Theory Manual Material Models 22.15 Material Model 15: Johnson and Cook Plasticity Model Johnson and Cook express the flow stress as 𝜎𝑦 = (𝐴 + 𝐵𝜀̅p𝑛 )(1 + 𝑐ln𝜀̇∗)(1 − 𝑇∗𝑚), (22.15.1) where 𝐴, 𝐵, 𝐶, 𝑛, and 𝑚 are user defined input constants, and: 𝜀̇∗ = = effective plastic strain rate for 𝜀̇0, in units of 𝜀̅𝑝 = effective plastic strain ̇𝑝 𝜀̅ 𝜀̇0 𝑇∗ = 𝑇 − 𝑇room 𝑇melt − 𝑇room [time] Constants for a variety of materials are provided in Johnson and Cook [1983]. Due to the nonlinearity in the dependence of flow stress on plastic strain, an accurate value of the flow stress requires iteration for the increment in plastic strain. However, by using a Taylor series expansion with linearization about the current time, we can solve for 𝜎𝑦 with sufficient accuracy to avoid iteration. The strain at fracture is given by 𝜀f = [𝐷1 + 𝐷2exp (𝐷3𝜎 ∗)][1 + 𝐷4ln𝜀∗][1 + 𝐷5𝑇∗], (22.15.2) where 𝐷𝑖, 𝑖 = 1, . . . ,5 are input constants and 𝜎 ∗ is the ratio of pressure divided by effective stress: 𝜎 ∗ = 𝜎eff . Fracture occurs when the damage parameter 𝐷 = ∑ Δ𝜀̅p 𝜀f reaches the value 1. (22.15.3) (22.15.4) A choice of three spall models is offered to represent material splitting, cracking, and failure under tensile loads. The pressure limit model limits the minimum hydrostatic pressure to the specified value, 𝑝 ≥ 𝑝min. If pressures more tensile than this limit are calculated, the pressure is reset to 𝑝min. This option is not strictly a spall model since the deviatoric stresses are unaffected by the pressure reaching the tensile cutoff and the pressure cutoff value 𝑝min remains unchanged throughout the analysis. The maximum principal stress spall model detects spall if the maximum principal stress, 𝜎max, exceeds the limiting value 𝜎p. Once spall is detected with this model, the deviatoric stresses are reset to zero and no hydrostatic tension is permitted. If tensile Material Models LS-DYNA Theory Manual pressures are calculated, they are reset to 0 in the spalled material. Thus, the spalled material behaves as rubble. The hydrostatic tension spall model detects spall if the pressure becomes more tensile than the specified limit, 𝑝min. Once spall is detected, the deviatoric stresses are set to zero and the pressure is required to be compressive. If hydrostatic tension is calculated then the pressure is reset to 0 for that element. In addition to the above failure criterion, this material model also supports a shell element deletion criterion based on the maximum stable time step size for the element, Δ𝑡max. Generally, Δ𝑡max goes down as the element becomes more distorted. To assure stability of time integration, the global LS-DYNA time step is the minimum of the Δ𝑡max values calculated for all elements in the model. Using this option allows the selective deletion of elements whose time step Δ𝑡max has fallen below the specified minimum time step, Δ𝑡crit. Elements which are severely distorted often indicate that material has failed and supports little load, but these same elements may have very small time steps and therefore control the cost of the analysis. This option allows these highly distorted elements to be deleted from the calculation, and, therefore, the analysis can proceed at a larger time step, and, thus, at a reduced cost. Deleted elements do not carry any load, and are deleted from all applicable slide surface definitions. Clearly, this option must be judiciously used to obtain accurate results at a minimum cost. Material type 15 is applicable to the high rate deformation of many materials including most metals. Unlike the Steinberg-Guinan model, the Johnson-Cook model remains valid down to lower strain rates and even into the quasistatic regime. Typical applications include explosive metal forming, ballistic penetration, and impact. LS-DYNA Theory Manual Material Models 22.16 Material Model 16: Pseudo Tensor This model can be used in two major modes - a simple tabular pressure- dependent yield surface, and a potentially complex model featuring two yield versus pressure functions with the means of migrating from one curve to the other. For both modes, load curve N1 is taken to be a strain rate multiplier for the yield strength. Note that this model must be used with equation-of-state type 8 or 9. Response Mode I. Tabulated Yield Stress Versus Pressure This model is well suited for implementing standard geologic models like the Mohr-Coulomb yield surface with a Tresca limit, as shown in Figure 22.16.1. Examples of converting conventional triaxial compression data to this type of model are found in (Desai and Siriwardane, 1984). Note that under conventional triaxial compression conditions, the LS-DYNA input corresponds to an ordinate of 𝜎1 − 𝜎3 rather than the more widely used , where 𝜎1 is the maximum principal stress and 𝜎3 is the minimum principal stress. 𝜎1−𝜎3 This material combined with equation-of-state type 9 (saturated) has been used very successfully to model ground shocks and soil-structure interactions at pressures up to 100kbar. To invoke Mode I of this model, set 𝑎0, 𝑎1, 𝑎2, 𝑎0f, and 𝑎1f to zero, The tabulated Mohr-Coulomb Tresca Friction Angle Cohesion Figure 22.16.1. Mohr-Coulomb surface with a Tresca limit. Material Models LS-DYNA Theory Manual values of pressure should then be specified on cards 4 and 5, and the corresponding values of yield stress should be specified on cards 6 and 7. The parameters relating to reinforcement properties, initial yield stress, and tangent modulus are not used in this response mode, and should be set to zero. Simple tensile failure Note that a1f is reset internally to 1/3 even though it is input as zero; this defines a material failure curve of slope 3𝑝, where p denotes pressure (positive in compression). In this case the yield strength is taken from the tabulated yield vs. pressure curve until the maximum principal stress (𝜎1) in the element exceeds the tensile cut-off (𝜎cut). For every time step that 𝜎1 > 𝜎cut the yield strength is scaled back by a fraction of the distance between the two curves until after 20 time steps the yield strength is defined by the failure curve. The only way to inhibit this feature is to set σcut arbitrarily large. Response Mode II. Two-Curve Model with Damage and Failure This approach uses two yield versus pressure curves of the form 𝜎y = 𝑎0 + 𝑎1 + 𝑎2𝑝 . (22.16.1) The upper curve is best described as the maximum yield strength curve and the lower curve is the material failure curve. There are a variety of ways of moving between the two curves and each is discussed below. MODE II.A: Simple tensile failure Define 𝑎0, 𝑎1, 𝑎2, 𝑎0f and 𝑎1f, set 𝑏1 to zero, and leave cards 4 through 7 blank. In this case the yield strength is taken from the maximum yield curve until the maximum principal stress (𝜎1) in the element exceeds the tensile cut-off (𝜎cut). For every time Figure 22.2. Two-curve concrete model with damage and failure. Pressure LS-DYNA Theory Manual Material Models step that 𝜎1 > 𝜎cut the yield strength is scaled back by a fraction of the distance between the two curves until after 20 time steps the yield strength is defined by the failure curve. Mode II.B: Tensile failure plus plastic strain scaling Define 𝑎0, 𝑎1, 𝑎2, 𝑎0f and 𝑎1f, set 𝑏1 to zero, and user cards 4 through 7 to define a scale factor, η, versus effective plastic strain. LS-DYNA evaluates η at the current effective plastic strain and then calculated the yield stress as 𝜎yield = 𝜎failed + 𝜂(𝜎max − 𝜎failed), (22.16.2) where 𝜎max and 𝜎failed are found as shown in Figure 19.16.2. This yield strength is then subject to scaling for tensile failure as described above. This type of model allows the description of a strain hardening or softening material such as concrete. Mode II.C: Tensile failure plus damage scaling The change in yield stress as a function of plastic strain arises from the physical mechanisms such as internal cracking, and the extent of this cracking is affected by the hydrostatic pressure when the cracking occurs. This mechanism gives rise to the "confinement" effect on concrete behavior. To account for this phenomenon, a "damage" function was defined and incorporated. This damage function is given the form: 𝜀p 𝜆 = ∫ (1 + 𝜎cut −𝑏1 ) 𝑑𝜀p . (22.16.3) Define 𝑎0, 𝑎1, 𝑎2, 𝑎0f and 𝑎1f, and 𝑏1. Cards 4 through 7 now give 𝜂 as a function of 𝜆 and scale the yield stress as 𝜎yield = 𝜎failed + 𝜂(𝜎max − 𝜎failed), (22.16.4) and then apply any tensile failure criteria. Mode II Concrete Model Options Material Type 16 Mode II provides the option of automatic internal generation of a simple "generic" model for concrete. If 𝑎0 is negative, then 𝜎cut is assumed to be the ′ and −𝑎0 is assumed to be a conversion unconfined concrete compressive strength, 𝑓c factor from LS-DYNA pressure units to psi. (For example, if the model stress units are MPa, 𝑎0 should be set to –145.) In this case the parameter values generated internally are Material Models LS-DYNA Theory Manual (22.16.5) 𝜎cut = 1.7 ′2 ⎜⎛ 𝑓c ⎟⎞ −𝑎0⎠ ⎝ 𝑎0 = 𝑎1 = ′ 𝑓c ′ 3𝑓c 𝑎0f = 0 𝑎1f = 0.385 𝑎2 = Note that these 𝑎0f and 𝑎1f defaults will be overwritten by non-zero entries on Card 3. If plastic strain or damage scaling is desired, Cards 5 through 8 and b1 should be specified in the input. When 𝑎0 is input as a negative quantity, the equation-of-state can be given as 0 and a trilinear EOS Type 8 model will be automatically generated from the unconfined compressive strength and Poisson's ratio. The EOS 8 model is a simple pressure versus volumetric strain model with no internal energy terms, and should give reasonable results for pressures up to 5kbar (approximately 72,500 psi). Mixture model A reinforcement fraction, 𝑓r, can be defined along with properties of the reinforcing material. The bulk modulus, shear modulus, and yield strength are then calculated from a simple mixture rule, i.e., for the bulk modulus the rule gives: 𝐾 = (1 − 𝑓r)𝐾m + 𝑓r𝐾r, (22.16.6) where 𝐾m and 𝐾r are the bulk moduli for the geologic material and the reinforcing material, respectively. This feature should be used with caution. It gives an isotropic effect in the material instead of the true anisotropic material behavior. A reasonable approach would be to use the mixture elements only where reinforcing material exists and plain elements elsewhere. When the mixture model is being used, the strain rate multiplier for the principal material is taken from load curve N1 and the multiplier for the reinforcement is taken from load curve N2. LS-DYNA Theory Manual Material Models 22.17 Material Model 17: Isotropic Elastic-Plastic With Oriented Cracks This is an isotropic elastic-plastic material which includes a failure model with an oriented crack. The von Mises yield condition is given by: 𝜎y where the second stress invariant, 𝐽2, is defined in terms of the deviatoric stress components as 𝜙 = 𝐽2 − (22.17.1) , 𝐽2 = 𝑠𝑖𝑗𝑠𝑖𝑗, (22.17.2) and the yield stress, 𝜎y, is a function of the effective plastic strain, 𝜀eff hardening modulus, 𝐸p: p , and the plastic p . 𝜎y = 𝜎0 + 𝐸p𝜀eff (22.17.3) The effective plastic strain is defined as: p = ∫ 𝑑𝜀eff 𝜀eff , (22.17.4) p = √2 where 𝑑𝜀eff input tangent modulus, 𝐸t, as 3 𝑑𝜀𝑖𝑗 p𝑑𝜀𝑖𝑗 p, and the plastic tangent modulus is defined in terms of the 𝐸p = 𝐸𝐸t 𝐸 − 𝐸t . (22.17.5) Pressure in this model is found from evaluating an equation of state. A pressure cutoff can be defined such that the pressure is not allowed to fall below the cutoff value. The oriented crack fracture model is based on a maximum principal stress criterion. When the maximum principal stress exceeds the fracture stress, 𝜎f, the element fails on a plane perpendicular to the direction of the maximum principal stress. The normal stress and the two shear stresses on that plane are then reduced to zero. This stress reduction is done according to a delay function that reduces the stresses gradually to zero over a small number of time steps. This delay function procedure is used to reduce the ringing that may otherwise be introduced into the system by the sudden fracture. Material Models LS-DYNA Theory Manual After a tensile fracture, the element will not support tensile stress on the fracture plane, but in compression will support both normal and shear stresses. The orientation of this fracture surface is tracked throughout the deformation, and is updated to If the maximum principal stress properly model finite deformation effects. subsequently exceeds the fracture stress in another direction, the element fails isotropically. In this case the element completely loses its ability to support any shear stress or hydrostatic tension, and only compressive hydrostatic stress states are possible. Thus, once isotropic failure has occurred, the material behaves like a fluid. This model is applicable to elastic or elastoplastic materials under significant tensile or shear loading when fracture is expected. Potential applications include brittle materials such as ceramics as well as porous materials such as concrete in cases where pressure hardening effects are not significant. LS-DYNA Theory Manual Material Models 22.18 Material Model 18: Power Law Isotropic Plasticity Elastoplastic behavior with isotropic hardening is provided by this model. The yield stress, 𝜎y, is a function of plastic strain and obeys the equation: 𝜎y = 𝑘𝜀𝑛 = 𝑘(𝜀yp + 𝜀̅p) , (22.18.1) where 𝜀yp is the elastic strain to yield and 𝜀̅p is the effective plastic strain (logarithmic). A parameter, SIGY, in the input governs how the strain to yield is identified. If SIGY is set to zero, the strain to yield if found by solving for the intersection of the linearly elastic loading equation with the strain hardening equation: which gives the elastic strain at yield as: 𝜎 = 𝐸𝜀, 𝜎 = 𝑘𝜀𝑛, 𝜀yp = ( 𝑛−1 . ) If SIGY yield is nonzero and greater than 0.02 then: 𝜀yp = ( 𝜎y . ) (22.18.2) (22.18.3) (22.18.4) Strain rate is accounted for using the Cowper-Symonds model which scales the yield stress with the factor 1 + ( P⁄ ) , 𝜀̇ (22.18.5) where 𝜀̇ is the strain rate. A fully viscoplastic formulation is optional with this model which incorporates the Cowper-Symonds formulation within the yield surface. An additional cost is incurred but the improvement allows for dramatic results. Material Models LS-DYNA Theory Manual 22.19 Material Model 19: Strain Rate Dependent Isotropic Plasticity In this model, a load curve is used to describe the yield strength 𝜎0 as a function of effective strain rate 𝜀̅ ̇ where 𝜀̅ ̇ = ( 2⁄ ′ ) ′ 𝜀̇𝑖𝑗 𝜀̇𝑖𝑗 , (22.19.1) and the prime denotes the deviatoric component. The yield stress is defined as ̇ ) + 𝐸p𝜀̅p. (22.19.2) where 𝜀̅p is the effective plastic strain and 𝐸p is given in terms of Young’s modulus and the tangent modulus by 𝜎y = 𝜎0(𝜀̅ 𝐸p = 𝐸𝐸t 𝐸 − 𝐸t . (22.19.3) Both Young's modulus and the tangent modulus may optionally be made functions of strain rate by specifying a load curve ID giving their values as a function of strain rate. If these load curve ID's are input as 0, then the constant values specified in the input are used. Note that all load curves used to define quantities as a function of strain rate must have the same number of points at the same strain rate values. This requirement is used to allow vectorized interpolation to enhance the execution speed of this constitutive model. This model also contains a simple mechanism for modeling material failure. This option is activated by specifying a load curve ID defining the effective stress at failure as a function of strain rate. For solid elements, once the effective stress exceeds the failure stress the element is deemed to have failed and is removed from the solution. For shell elements the entire shell element is deemed to have failed if all integration points through the thickness have an effective stress that exceeds the failure stress. After failure the shell element is removed from the solution. In addition to the above failure criterion, this material model also supports a shell element deletion criterion based on the maximum stable time step size for the element, Δ𝑡max. Generally, Δ𝑡max goes down as the element becomes more distorted. To assure stability of time integration, the global LS-DYNA time step is the minimum of the Δ𝑡max values calculated for all elements in the model. Using this option allows the selective deletion of elements whose time step Δ𝑡max has fallen below the specified minimum time step, Δ𝑡crit. Elements which are severely distorted often indicate that LS-DYNA Theory Manual Material Models material has failed and supports little load, but these same elements may have very small time steps and therefore control the cost of the analysis. This option allows these highly distorted elements to be deleted from the calculation, and, therefore, the analysis can proceed at a larger time step, and, thus, at a reduced cost. Deleted elements do not carry any load, and are deleted from all applicable slide surface definitions. Clearly, this option must be judiciously used to obtain accurate results at a minimum cost. Material Models LS-DYNA Theory Manual 22.20 Material Model 20: Rigid The rigid material type 20 provides a convenient way of turning one or more parts comprised of beams, shells, or solid elements into a rigid body. Approximating a deformable body as rigid is a preferred modeling technique in many real world applications. For example, in sheet metal forming problems the tooling can properly and accurately be treated as rigid. In the design of restraint systems the occupant can, for the purposes of early design studies, also be treated as rigid. Elements which are rigid are bypassed in the element processing and no storage is allocated for storing history variables; consequently, the rigid material type is very cost efficient. Two unique rigid part IDs may not share common nodes unless they are merged together using the rigid body merge option. A rigid body may be made up of disjoint finite element meshes, however. LS-DYNA assumes this is the case since this is a common practice in setting up tooling meshes in forming problems. All elements which reference a given part ID corresponding to the rigid material should be contiguous, but this is not a requirement. If two disjoint groups of elements on opposite sides of a model are modeled as rigid, separate part ID's should be created for each of the contiguous element groups if each group is to move independently. This requirement arises from the fact that LS-DYNA internally computes the six rigid body degrees-of-freedom for each rigid body (rigid material or set of merged materials), and if disjoint groups of rigid elements use the same part ID, the disjoint groups will move together as one rigid body. Inertial properties for rigid materials may be defined in either of two ways. By default, the inertial properties are calculated from the geometry of the constituent elements of the rigid material and the density specified for the part ID. Alternatively, the inertial properties and initial velocities for a rigid body may be directly defined, and this overrides data calculated from the material property definition and nodal initial velocity definitions. Young's modulus, E, and Poisson's ratio, υ are used for determining sliding interface parameters if the rigid body interacts in a contact definition. Realistic values for these constants should be defined since unrealistic values may contribute to numerical problem in contact. LS-DYNA Theory Manual Material Models 22.21 Material Model 21: Thermal Orthotropic Elastic In the implementation for three-dimensional continua a total Lagrangian formulation is used. In this approach the material law that relates second Piola- Kirchhoff stress 𝐒 to the Green-St. Venant strain 𝐄 is 𝐒 = 𝐂 ⋅ 𝐄 = 𝐓T𝐂l𝐓 ⋅ 𝐄, where 𝐓 is the transformation matrix [Cook 1974]. 𝐓 = 𝑙1 ⎡ ⎢ 𝑙2 ⎢ ⎢ 𝑙3 ⎢ ⎢ 2𝑙1𝑙2 ⎢ 2𝑙2𝑙3 ⎢ 2𝑙3𝑙1 ⎣ 𝑚1 𝑚2 𝑚3 2𝑚1𝑚2 2𝑚2𝑚3 2𝑚3𝑚1 𝑛1 𝑛2 𝑛3 2𝑛1𝑛2 2𝑛2𝑛3 2𝑛3𝑛1 𝑙1𝑚1 𝑙2𝑚2 𝑙3𝑚3 (𝑙1𝑚2 + 𝑙2𝑚1) (𝑙2𝑚3 + 𝑙3𝑚2) (𝑙3𝑚1 + 𝑙1𝑚3) 𝑚1𝑛1 𝑚2𝑛2 𝑚3𝑛3 (𝑚1𝑛2 + 𝑚2𝑛1) (𝑚2𝑛3 + 𝑚3𝑛2) (𝑚3𝑛1 + 𝑚1𝑛3) 𝑛1𝑙1 ⎤ ⎥ 𝑛2𝑙2 ⎥ ⎥ 𝑛3𝑙3 , ⎥ ⎥ (𝑛1𝑙2 + 𝑛2𝑙1) ⎥ (𝑛2𝑙3 + 𝑛3𝑙2) ⎥ (𝑛3𝑙1 + 𝑛1𝑙3)⎦ 𝑙𝑖, 𝑚𝑖, 𝑛𝑖 are the direction cosines (22.21.1) (22.21.2) (22.21.3) ′ denotes the material axes. The constitutive matrix 𝐂l is defined in terms of the ′ = 𝑙𝑖𝑥1 + 𝑚𝑖𝑥2 + 𝑛𝑖𝑥3 for 𝑖 = 1, 2, 3, 𝑥𝑖 and 𝑥𝑖 material axes as −1 = 𝐂l 𝐸11 𝜐12 𝐸 11 𝜐13 𝐸11 − − − − 𝜐21 𝐸22 𝐸22 𝜐23 𝐸22 − − 𝜐31 𝐸33 𝜐32 𝐸33 𝐸33 ⎡ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎣ 𝐺12 𝐺23 ⎤ ⎥ ⎥ ⎥ ⎥ ⎥ ⎥ ⎥ ⎥ , ⎥ ⎥ ⎥ ⎥ ⎥ ⎥ ⎥ ⎥ 𝐺31⎦ (22.21.4) where the subscripts denote the material axes, i.e., υ𝑖𝑗 = υ𝑥′𝑖 𝑥′𝑗 and 𝐸𝑖𝑖 = 𝐸𝑥′𝑖. (22.21.5) Since 𝐂l is symmetric υ12 𝐸11 = υ21 𝐸22 , etc. (22.21.6) Material Models LS-DYNA Theory Manual The vector of Green-St. Venant strain components is 𝐄T = [𝐸11 𝐸22 𝐸33 𝐸12 𝐸23 𝐸31], which include the local thermal strains which are integrated in time: 𝑛+1 = 𝜀𝑎𝑎 𝜀𝑎𝑎 𝑛+1 = 𝜀𝑏𝑏 𝜀𝑏𝑏 𝑛+1 = 𝜀𝑐𝑐 𝜀𝑐𝑐 𝑛 + 𝛼𝑎(𝑇𝑛+1 − 𝑇𝑛), 𝑛 + 𝛼𝑏(𝑇𝑛+1 − 𝑇𝑛), 𝑛 + 𝛼𝑐(𝑇𝑛+1 − 𝑇𝑛). (22.21.7) (22.21.8) After computing 𝑆𝑖𝑗 we use Equation (18.32) to obtain the Cauchy stress. This model will predict realistic behavior for finite displacement and rotations as long as the strains are small. For shell elements, the stresses are integrated in time and are updated in the corotational coordinate system. In this procedure the local material axes are assumed to remain orthogonal in the deformed configuration. This assumption is valid if the strains remain small. LS-DYNA Theory Manual Material Models 22.22 Material Model 22: Chang-Chang Composite Failure Model For shells, five material parameters are used in the three failure criteria. These are [Chang and Chang 1987a, 1987b]: • 𝑆1, longitudinal tensile strength • 𝑆2, transverse tensile strength • 𝑆12, shear strength • 𝐶2, transverse compressive strength • 𝛼, nonlinear shear stress parameter. 𝑆1, 𝑆2, 𝑆12, and 𝐶2 are obtained from material strength measurement. 𝛼 is defined by material shear stress-strain measurements. In plane stress, the strain is given in terms of the stress as (𝜎1 − 𝜐1𝜎2), (𝜎2 − 𝜐2𝜎1), (22.22.1) 𝜀1 = 𝜀2 = 𝐸1 𝐸2 2𝜀12 = 3 . 𝜏12 + 𝛼𝜏12 𝐺12 The third equation defines the nonlinear shear stress parameter 𝛼. A fiber matrix shearing term augments each damage mode: 𝜏̅ = 𝜏12 2𝐺12 𝑆12 2𝐺12 + 3 + 3 𝛼𝜏12 𝛼𝑆12 , which is the ratio of the shear stress to the shear strength. The matrix cracking failure criteria is determined from 𝐹matrix = ( ) 𝜎2 𝑆2 + 𝜏̅, (22.22.2) (22.22.3) where failure is assumed whenever 𝐹matrix > 1. If 𝐹matrix > 1, then the material constants 𝐸2, 𝐺12, 𝜐1, and 𝜐2 are set to zero. The compression failure criteria is given as Material Models LS-DYNA Theory Manual 𝐹comp = ( 𝜎2 2𝑆12 ) + ) 𝐶2 2𝑆12 ⎢⎡( ⎣ − 1 ⎥⎤ 𝜎2 𝐶2 ⎦ + 𝜏̅, (22.22.4) where failure is assumed whenever 𝐹comb > 1. If 𝐹comb > 1, then the material constants 𝐸2, 𝜐1, and 𝜐2 are set to zero. The final failure mode is due to fiber breakage. 𝐹fiber = ( ) 𝜎1 S1 + 𝜏̅, (22.22.5) Failure is assumed whenever 𝐹fiber > 1. If 𝐹fiber > 1, then the constants 𝐸1, 𝐸2, 𝐺12 𝜐1 and 𝜐2 are set to zero. For solids, a fourth failure mode corresponding to delamination is computed as 𝐹delam = ( max (0.0, 𝜎3) S3 ) + ( ) 𝜏23 S23 + ( ) 𝜏31 S31 This involves three additional material parameters. • 𝑆3, normal tensile strength • 𝑆23, transverse shear strength • 𝑆31, transverse shear strength (22.22.140) LS-DYNA Theory Manual Material Models 22.23 Material Model 23: Thermal Orthotropic Elastic with 12 Curves In the implementation for three-dimensional continua a total Lagrangian formulation is used. In this approach the material law that relates second Piola- Kirchhoff stress 𝐒 to the Green-St. Venant strain 𝐄 is 𝐒 = 𝐂 ⋅ 𝐄 = 𝐓T𝐂l𝐓 ⋅ 𝐄, where 𝐓 is the transformation matrix [Cook 1974]. 𝐓 = 𝑙1 ⎡ ⎢ 𝑙2 ⎢ ⎢ 𝑙3 ⎢ ⎢ 2𝑙1𝑙2 ⎢ 2𝑙2𝑙3 ⎢ 2𝑙3𝑙1 ⎣ 𝑚1 𝑚2 𝑚3 2𝑚1𝑚2 2𝑚2𝑚3 2𝑚3𝑚1 𝑙𝑖, 𝑚𝑖, 𝑛𝑖 are the direction cosines 𝑛1 𝑛2 𝑛3 2𝑛1𝑛2 2𝑛2𝑛3 2𝑛3𝑛1 𝑙1𝑚1 𝑙2𝑚2 𝑙3𝑚3 (𝑙1𝑚2 + 𝑙1𝑚1) (𝑙2𝑚3 + 𝑙3𝑚2) (𝑙3𝑚1 + 𝑙1𝑚3) 𝑚1𝑛1 𝑚2𝑛2 𝑚3𝑛3 (𝑚1𝑛2 + 𝑚2𝑛1) (𝑚2𝑛3 + 𝑚3𝑛2) (𝑚3𝑛1 + 𝑚1𝑛3) 𝑛1𝑙1 ⎤ ⎥ 𝑛2𝑙2 ⎥ ⎥ 𝑛3𝑙3 ⎥ ⎥ (𝑛1𝑙2 + 𝑛2𝑙1) ⎥ (𝑛2𝑙3 + 𝑛3𝑙2) ⎥ (𝑛3𝑙1 + 𝑛1𝑙3)⎦ , (22.23.1) (22.23.2) (22.23.3) ′ denotes the material axes. The temperature dependent constitutive matrix 𝐂l is ′ = 𝑙𝑖𝑥1 + 𝑚𝑖𝑥2 + 𝑛𝑖𝑥3 𝑥𝑖 for 𝑖 = 1, 2, 3, and 𝑥𝑖 defined in terms of the material axes as −1 = 𝐂l 𝐸11(𝑇) 𝜐12(𝑇) 𝐸11(𝑇) 𝜐13(𝑇) 𝐸11(𝑇) − − − − 𝜐21(𝑇) 𝐸22(𝑇) 𝐸22(𝑇) 𝜐23(𝑇) 𝐸 22(𝑇) − − 𝜐31(𝑇) 𝐸33(𝑇) 𝜐32(𝑇) 𝐸33(𝑇) 𝐸33(𝑇) ⎡ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎣ 𝐺12(𝑇) 𝐺23(𝑇) ⎤ ⎥ ⎥ ⎥ ⎥ ⎥ ⎥ ⎥ ⎥ , ⎥ ⎥ ⎥ ⎥ ⎥ ⎥ ⎥ ⎥ 𝐺31(𝑇)⎦ (22.23.4) where the subscripts denote the material axes, i.e., 𝜐𝑖𝑗 = υ𝑥′𝑖 𝑥′𝑗 and 𝐸𝑖𝑖 = 𝐸𝑥′𝑖. (22.23.5) Since 𝐂l is symmetric 𝜐12 𝐸11 = 𝜐21 𝐸22 , etc. (22.23.6) Material Models LS-DYNA Theory Manual The vector of Green-St. Venant strain components is 𝐄T = [𝐸11 𝐸22 𝐸33 𝐸12 𝐸23 𝐸31], which include the local thermal strains which are integrated in time: 𝑛+1 = 𝜀𝑎𝑎 𝜀𝑎𝑎 𝑛 + 𝛼𝑎 (𝑇 𝑛+1 2) [𝑇𝑛+1 − 𝑇𝑛], 𝑛+1 = 𝜀𝑏𝑏 𝜀𝑏𝑏 𝑛 + 𝛼𝑏 (𝑇 𝑛+1 2) [𝑇𝑛+1 − 𝑇𝑛], 𝑛+1 = 𝜀𝑐𝑐 𝜀𝑐𝑐 𝑛 + 𝛼𝑐 (𝑇 𝑛+1 2) [𝑇𝑛+1 − 𝑇𝑛]. (22.23.7) (22.23.8) After computing 𝑆𝑖𝑗 we use Equation (16.32) to obtain the Cauchy stress. This model will predict realistic behavior for finite displacement and rotations as long as the strains are small. For shell elements, the stresses are integrated in time and are updated in the corotational coordinate system. In this procedure the local material axes are assumed to remain orthogonal in the deformed configuration. This assumption is valid if the strains remain small. LS-DYNA Theory Manual Material Models 22.24 Material Model 24: Piecewise Linear Isotropic Plasticity This plasticity treatment in this model is quite similar to Model 10, but unlike 10, it includes strain rate effects and does not use an equation of state. Deviatoric stresses are determined that satisfy the yield function 𝜙 = 𝑠𝑖𝑗𝑠𝑖𝑗 − 𝜎y ≤ 0, (22.24.1) where where the hardening function 𝑓h(𝜀eff Otherwise, linear hardening of the form σy = 𝛽[𝜎0 + 𝑓h(𝜀eff (22.24.2) p ) can be specified in tabular form as an option. p )], p ) = 𝐸p(𝜀eff p ), 𝑓h(𝜀eff (22.24.3) p are given in Equations (22.3.6) and (8.61), respectively. is assumed where 𝐸p and 𝜀eff The parameter 𝛽 accounts for strain rate effects. For complete generality a table defining the yield stress versus plastic strain may be defined for various levels of effective strain rate. In the implementation of this material model, the deviatoric stresses are updated elastically , the yield function is checked, and if it is satisfied the deviatoric stresses are accepted. If it is not, an increment in plastic strain is computed: p = Δ𝜀eff (3 2⁄ ∗ ) ∗ 𝑠𝑖𝑗 𝑠𝑖𝑗 3𝐺 + 𝐸p − 𝜎y , (22.24.4) is the shear modulus and 𝐸p is the current plastic hardening modulus. The trial deviatoric stress state 𝑠𝑖𝑗 ∗ is scaled back: 𝑛+1 = 𝑠𝑖𝑗 𝜎𝑦 2⁄ ∗ ) ∗ 𝑠𝑖𝑗 𝑠𝑖𝑗 (3 ∗ . 𝑠𝑖𝑗 (22.24.5) For shell elements, the above equations apply, but with the addition of an iterative loop to solve for the normal strain increment, such that the stress component normal to the mid surface of the shell element approaches zero. Three options to account for strain rate effects are possible: Material Models LS-DYNA Theory Manual 1. Strain rate may be accounted for using the Cowper-Symonds model which scales the yield stress with the factor 𝛽 = 1 + ( 𝑝⁄ ) . 𝜀̇ (22.24.6) where 𝜀̇ is the strain rate. 2. 3. For complete generality a load curve, defining 𝛽, which scales the yield stress may be input instead. In this curve the scale factor versus strain rate is de- fined. If different stress versus strain curves can be provided for various strain rates, the option using the reference to a table definition can be used. See Fig- ure 19.24.1. A fully viscoplastic formulation is optional which incorporates the different options above within the yield surface. An additional cost is incurred over the simple scaling but the improvement is results can be dramatic. If a table ID is specified a curve ID is given for each strain rate, see Section 23. Intermediate values are found by interpolating between curves. Effective plastic strain versus yield stress is expected. If the strain rate values fall out of range, extrapolation is not used; rather, either the first or last curve determines the yield stress depending on whether the rate is low or high, respectively. LS-DYNA Theory Manual Material Models 22.25 Material Model 25: Kinematic Hardening Cap Model The implementation of an extended two invariant cap model, suggested by Stojko [1990], is based on the formulations of Simo, et al. [1988, 1990] and Sandler and Rubin [1979]. In this model, the two invariant cap theory is extended to include nonlinear kinematic hardening as suggested by Isenberg, Vaughn, and Sandler [1978]. A brief discussion of the extended cap model and its parameters is given below. The cap model is formulated in terms of the invariants of the stress tensor. The square root of the second invariant of the deviatoric stress tensor, √𝐽2D is found from the deviatoric stresses 𝐒 as √𝐽2D ≡ √ 𝑠𝑖𝑗𝑠𝑖𝑗, (22.25.1) and is the objective scalar measure of the distortional or shearing stress. The first invariant of the stress, 𝐽1, is the trace of the stress tensor. The cap model consists of three surfaces in √𝐽2D − 𝐽1 space, as shown in Figure 22.25.1. First, there is a failure envelope surface, denoted 𝑓1 in the figure. The functional form of 𝑓1 is where 𝐹e is given by 𝑓1 = √𝐽2D − min(𝐹e(𝐽1), 𝑇mises), 𝐹e(𝐽1) ≡ 𝛼 − 𝛾exp(−𝛽𝐽1) + 𝜃𝐽1. (22.25.2) (22.25.3) εp eff Figure 22.25.1. Rate effects may be accounted for by defining a table of curves. Material Models LS-DYNA Theory Manual 2D J = Fe 2D f1 f3 J = Fc 2D f2 J1 X( ) Figure 22.25.2. The yield surface of the two-invariant cap model in pressure √𝐽2D − 𝐽1 space Surface 𝑓1 is the failure envelope, 𝑓2 is the cap surface, and 𝑓3 is the tension cutoff. and 𝑇mises ≡ |𝑋(𝜅𝑛) − 𝐿(𝜅𝑛)|. This failure envelope surface is fixed in √𝐽2D − 𝐽1 space, and therefore does not harden unless kinematic hardening is present. Next, there is a cap surface, denoted 𝑓2 in the figure, with 𝑓2 given by where 𝐹c is defined by 𝑓2 = √𝐽2D − 𝐹c(𝐽1, 𝜅), 𝑋(𝜅) is the intersection of the cap surface with the 𝐽1 axis √[𝑋(𝜅) − 𝐿(𝜅)] 2 − [𝐽1 − 𝐿(𝜅)] 2, 𝐹c(𝐽1, 𝜅) ≡ and 𝐿(𝜅) is defined by 𝑋(𝜅) = 𝜅 + 𝑅𝐹e(𝜅), 𝐿(𝜅) ≡ { 𝜅 > 0 0 𝜅 ≤ 0 . (22.25.4) (22.25.5) (22.25.6) (22.25.7) The hardening parameter 𝜅 is related to the plastic volume change 𝜀v p through the hardening law p = W{1 − exp[−𝐷(𝑋(κ) − 𝑋0)]}. 𝜀v (22.25.8) Geometrically, 𝜅 is seen in the figure as the 𝐽1 coordinate of the intersection of the cap surface and the failure surface. Finally, there is the tension cutoff surface, denoted 𝑓3 in the figure. The function 𝑓3 is given by 𝑓3 + 𝑇 − 𝐽1, (22.25.9) where 𝑇 is the input material parameter which specifies the maximum hydrostatic tension sustainable by the material. The elastic domain in √𝐽2D − 𝐽1 space is then LS-DYNA Theory Manual Material Models bounded by the failure envelope surface above, the tension cutoff surface on the left, and the cap surface on the right. An additive decomposition of the strain into elastic and plastic parts is assumed: (22.25.10) where 𝜀e is the elastic strain and 𝜀p is the plastic strain. Stress is found from the elastic strain using Hooke’s law, 𝜀 = 𝜀 + 𝜀P, 𝜎 = 𝐶(𝜀 − 𝜀P), (22.25.11) where 𝜎 is the stress and 𝐶 is the elastic constitutive tensor. The yield condition may be written 𝑓1(𝜎) ≤ 0, 𝑓2(𝜎, 𝜅) ≤ 0, 𝑓3(𝜎) ≤ 0, and the plastic consistency condition requires that 𝜆̇𝑘𝑓𝑘 = 0 𝜆̇𝑘 ≥ 0 𝑘 = 1, 2, 3, (22.25.12) (22.25.13) where 𝜆𝑘 is the plastic consistency parameter for surface 𝑘. If 𝑓𝑘 < 0, then 𝜆̇𝑘 = 0 and the response is elastic. If 𝑓𝑘 > 0, then surface k is active and 𝜆̇𝑘 is found from the requirement that 𝑓 ̇ 𝑘 = 0. Associated plastic flow is assumed, so using Koiter’s flow rule the plastic strain rate is given as the sum of contribution from all of the active surfaces, 𝜀̇p = ∑ 𝜆̇𝑘 𝑘=1 ∂𝑓𝑘 ∂𝑠 . (22.25.14) One of the major advantages of the cap model over other classical pressure- dependent plasticity models is the ability to control the amount of dilatency produced under shear loading. Dilatency is produced under shear loading as a result of the yield surface having a positive slope in √𝐽2D − 𝐽1 space, so the assumption of plastic flow in the direction normal to the yield surface produces a plastic strain rate vector that has a component in the volumetric (hydrostatic) direction . In models such as the Drucker-Prager and Mohr-Coulomb, this dilatency continues as long as shear loads are applied, and in many cases produces far more dilatency than is experimentally observed in material tests. In the cap model, when the failure surface is active, dilatency is produced just as with the Drucker-Prager and Mohr-Columb models. However, the hardening law permits the cap surface to contract until the cap intersects the failure envelope at the stress point, and the cap remains at that point. The local normal to the yield surface is now vertical, and therefore the normality rule assures that no further plastic volumetric strain (dilatency) is created. Adjustment of Material Models LS-DYNA Theory Manual the parameters that control the rate of cap contractions permits experimentally observed amounts of dilatency to be incorporated into the cap model, thus producing a constitutive law which better represents the physics to be modeled. Another advantage of the cap model over other models such as the Drucker-Prager and Mohr-Coulomb is the ability to model plastic compaction. In these models all purely volumetric response is elastic. In the cap model, volumetric response is elastic until the stress point hits the cap surface. Therefore, plastic volumetric strain (compaction) is generated at a rate controlled by the hardening law. Thus, in addition to controlling the amount of dilatency, the introduction of the cap surface adds another experimentally observed response characteristic of geological material into the model. The inclusion of kinematic hardening results in hysteretic energy dissipation under cyclic loading conditions. Following the approach of Isenberg, et al., [1978] a nonlinear kinematic hardening law is used for the failure envelope surface when nonzero values of and N are specified. In this case, the failure envelope surface is replaced by a family of yield surfaces bounded by an initial yield surface and a limiting failure envelope surface. Thus, the shape of the yield surfaces described above remains unchanged, but they may translate in a plane orthogonal to the J axis. Translation of the yield surfaces is permitted through the introduction of a “back stress” tensor, α. The formulation including kinematic hardening is obtained by replacing the stress σ with the translated stress tensor 𝜂 ≡ 𝜎 − 𝛼 in all of the above equation. The history tensor α is assumed deviatoric, and therefore has only 5 unique components. The evolution of the back stress tensor is governed by the nonlinear hardening law (22.25.15) where c̅ is a constant, 𝐹̅ is a scalar function of 𝜎 and 𝛼 and 𝜀̇p is the rate of deviator plastic strain. The constant may be estimated from the slope of the shear stress - plastic shear strain curve at low levels of shear stress. 𝛼 = c̅𝐹̅(𝜎, 𝛼) 𝜀̇p, The function 𝐹̅ is defined as 𝐹̅ ≡ max (0,1 − (𝜎 − 𝛼)𝛼 2N𝐹𝑒(𝐽1) ), (22.25.16) where N is a constant defining the size of the yield surface. The value of N may be interpreted as the radial distant between the outside of the initial yield surface and the inside of the limit surface. In order for the limit surface of the kinematic hardening cap model to correspond with the failure envelope surface of the standard cap model, the scalar parameter a must be replaced α − N in the definition 𝐹e. The cap model contains a number of parameters which must be chosen to represent a particular material, and are generally based on experimental data. The parameters 𝛼, 𝛽, 𝜃 and 𝛾 are usually evaluated by fitting a curve through failure data taken from a set of triaxial compression tests. The parameters 𝑊, 𝐷, and X0 define the LS-DYNA Theory Manual Material Models cap hardening law. The value W represents the void fraction of the uncompressed sample and 𝐷 governs the slope of the initial loading curve in hydrostatic compression. The value of R is the ration of major to minor axes of the quarter ellipse defining the cap surface. Additional details and guidelines for fitting the cap model to experimental data are found in [Chen and Baladi, 1985]. Material Models LS-DYNA Theory Manual 22.26 Material Model 26: Crushable Foam This orthotropic material model does the stress update in the local material system denoted by the subscripts, 𝑎, 𝑏, and 𝑐. The material model requires the following input parameters: • E, Young’s modulus for the fully compacted material; • 𝜈, Poisson’s ratio for the compacted material; • 𝜎y, yield stress for fully compacted honeycomb; • LCA, load curve number for sigma-aa versus either relative volume or volumet- ric strain ; • LCB, load curve number for sigma-bb versus either relative volume or volumet- ric strain (default: LCB = LCA); • LCC, the load curve number for sigma-cc versus either relative volume or volumetric strain (default: LCC = LCA); • LCS, the load curve number for shear stress versus either relative volume or volumetric strain (default LCS = LCA); • 𝑉f, relative volume at which the honeycomb is fully compacted; • 𝐸𝑎𝑎u, elastic modulus in the uncompressed configuration; • 𝐸𝑏𝑏u, elastic modulus in the uncompressed configuration; • 𝐸𝑐𝑐u, elastic modulus in the uncompressed configuration; • 𝐺𝑎𝑏u, elastic shear modulus in the uncompressed configuration; • 𝐺𝑏𝑐u, elastic shear modulus in the uncompressed configuration; • 𝐺𝑐𝑎u, elastic shear modulus in the uncompressed configuration; • LCAB, load curve number for sigma-ab versus either relative volume or volumetric strain (default: LCAB = LCS); • LCBC, load curve number for sigma-bc versus either relative volume or volumetric strain default: LCBC = LCS); • LCCA, load curve number for sigma-ca versus either relative volume or volumetric strain (default: LCCA = LCS); • LCSR, optional load curve number for strain rate effects. The behavior before compaction is orthotropic where the components of the stress tensor are uncoupled, i.e., an 𝑎 component of strain will generate resistance in the local 𝑎 direction with no coupling to the local 𝑏 and 𝑐 directions. The elastic moduli (22.26.1) (22.26.2) (22.26.3) LS-DYNA Theory Manual Material Models vary linearly with the relative volume from their initial values to the fully compacted values: 𝐸𝑎𝑎 = 𝐸𝑎𝑎u + 𝛽(𝐸 − 𝐸𝑎𝑎u), 𝐸𝑏𝑏 = 𝐸𝑏𝑏u + 𝛽(𝐸 − 𝐸𝑏𝑏u), 𝐸𝑐𝑐 = 𝐸𝑐𝑐u + 𝛽(𝐸 − 𝐸𝑐𝑐u), 𝐺𝑎𝑏 = 𝐺𝑎𝑏u + 𝛽(𝐺 − 𝐺𝑎𝑏u), 𝐺𝑏𝑐 = 𝐺𝑏𝑐u + 𝛽(𝐺 − 𝐺𝑏𝑐u), 𝐺𝑐𝑎 = 𝐺𝑐𝑎u + 𝛽(𝐺 − 𝐺𝑐𝑎u), 𝛽 = max [min ( 1 − 𝑉min 1 − 𝑉𝑓 , 1) ,0], where and 𝐺 is the elastic shear modulus for the fully compacted honeycomb material 𝐺 = 2(1 + 𝜈) . The relative volume V is defined as the ratio of the current volume over the initial volume; typically, 𝑉 = 1 at the beginning of a calculation. The relative volume, 𝑉min, is the minimum value reached during the calculation. The load curves define the magnitude of the average stress as the material changes density (relative volume). Each curve related to this model must have the same Curve extends into negative volumetric strain quadrant since LS-DYNA will extrapolate using the two end points. It is important that the extropolation does not extend into the negative stress region. ij unloading and reloading path strain: -ε ij Unloading is based on the interpolated Young’s moduli which must provide an unloading tangent that exceeds the loading tangent. Figure 22.26.1. Stress quantity versus volumetric strain. Note that the “yield stress” at a volumetric strain of zero is nonzero. In the load curve definition, the “time” value is the volumetric strain and the “function” value is the yield stress. Material Models LS-DYNA Theory Manual number of points and the same abscissa values. There are two ways to define these curves: as a function of relative volume V, or as a function of volumetric strain defined as: 𝜀𝑉 = 1 − 𝑉. (22.26.4) In the former, the first value in the curve should correspond to a value of relative volume slightly less than the fully compacted value. In the latter, the first value in the curve should be less than or equal to zero corresponding to tension and should increase to full compaction. When defining the curves, care should be taken that the extrapolated values do not lead to negative yield stresses. At the beginning of the stress update we transform each element’s stresses and strain rates into the local element coordinate system. For the uncompacted material, the trial stress components are updated using the elastic interpolated moduli according to: 𝑛+1trial 𝑛+1trial 𝑛+1trial 𝑛+1trial 𝑛+1trial 𝑛+1trial 𝜎𝑎𝑎 𝜎𝑏𝑏 𝜎𝑐𝑐 𝜎𝑎𝑏 𝜎𝑏𝑐 𝜎𝑐𝑎 = 𝜎𝑎𝑎 = 𝜎𝑏𝑏 = 𝜎𝑐𝑐 = 𝜎𝑎𝑏 = 𝜎𝑏𝑐 = 𝜎𝑐𝑎 𝑛 + 𝐸𝑎𝑎Δ𝜀𝑎𝑎, 𝑛 + 𝐸𝑏𝑏Δ𝜀𝑏𝑏, 𝑛 + 𝐸𝑐𝑐Δ𝜀𝑐𝑐, 𝑛 + 2𝐺𝑎𝑏Δ𝜀𝑎𝑏, 𝑛 + 2𝐺𝑏𝑐Δ𝜀𝑏𝑐, 𝑛 + 2𝐺𝑐𝑎Δ𝜀𝑐𝑎 = 1. (22.26.5) Then we independently check each component of the updated stresses to ensure that they do not exceed the permissible values determined from the load curves, e.g., if then 𝑛+1trial ∣𝜎𝑖𝑗 ∣ > 𝜆𝜎𝑖𝑗(𝑉min), 𝑛+1 = 𝜎𝑖𝑗(𝑉min) 𝜎𝑖𝑗 𝑛+1trial 𝜆𝜎𝑖𝑗 𝑛+1trial∣ ∣𝜎𝑖𝑗 . (22.26.6) (22.26.7) The parameter 𝜆 is either unity or a value taken from the load curve number, LCSR, that defines 𝜆 as a function of strain rate. Strain rate is defined here as the Euclidean norm of the deviatoric strain rate tensor. For fully compacted material we assume that the material behavior is elastic- perfectly plastic and updated the stress components according to trial = 𝑠𝑖𝑗 𝑠𝑖𝑗 𝑛 + 2𝐺Δ𝜀𝑖𝑗 dev𝑛+1 2⁄ , (22.26.8) where the deviatoric strain increment is defined as LS-DYNA Theory Manual Material Models Δ𝜀𝑖𝑗 dev = Δ𝜀𝑖𝑗 − Δ𝜀𝑘𝑘𝛿𝑖𝑗. (22.26.9) We next check to see if the yield stress for the fully compacted material is exceeded by comparing trial = ( 𝑠eff 2⁄ trial) trial𝑠𝑖𝑗 𝑠𝑖𝑗 . (22.26.10) the effective trial stress, to the yield stress 𝜎y. If the effective trial stress exceeds the yield stress, we simply scale back the stress components to the yield surface: 𝑛+1 = 𝑠𝑖𝑗 𝜎y trial 𝑠eff trial. 𝑠𝑖𝑗 We can now update the pressure using the elastic bulk modulus, 𝐾: 2⁄ 𝑛+1 𝑝𝑛+1 = 𝑝𝑛 − 𝐾Δ𝜀𝑘𝑘 , 3(1 − 2𝜈) 𝐾 = , and obtain the final value for the Cauchy stress 𝑛+1 = 𝑠𝑖𝑗 𝜎𝑖𝑗 𝑛+1 − 𝑝𝑛+1𝛿𝑖𝑗. (22.26.11) (22.26.12) (22.26.13) After completing the stress update, we transform the stresses back to the global configuration. Material Models LS-DYNA Theory Manual 22.27 Material Model 27: Incompressible Mooney-Rivlin Rubber The Mooney-Rivlin material model is based on a strain energy function, 𝑊, as follows 𝑊 = A(𝐼1 − 3) + B(𝐼2 − 3) + C( 2 − 1) + D(𝐼3 − 1)2. 𝐼3 (22.27.1) A and B are user defined constants, whereas C and D are related to A and B as follows C = D = A + B, A(5𝜐 − 2) + B(11𝜐 − 5) 2(1 − 2𝜐) . (22.27.2) The derivation of the constants C and D is straightforward [Feng, 1993] and is included here since we were unable to locate it in the literature. The principal components of Cauchy stress, 𝜎𝑖, are given by [Ogden, 1984] For uniform dilation 𝐽𝜎𝑖 = 𝜆𝑖 ∂𝑊 ∂𝜆𝑖 . 𝜆1 = 𝜆2 = 𝜆3 = 𝜆, thus the pressure, 𝑝, is obtained (please note the sign convention), 𝑝 = 𝜎1 = 𝜎2 = 𝜎3 = 𝜆3 (𝜆2 𝜕𝑊 𝜕𝐼1 + 2𝜆4 𝜕𝑊 𝜕𝐼2 + 𝜆6 𝜕𝑊 𝜕𝐼3 ). The relative volume, 𝑉, can be defined in terms of the stretches as: 𝑉 = 𝜆3 = new volume old volume . (22.27.3) (22.27.4) (22.27.5) (22.27.6) For small volumetric deformations the bulk modulus, 𝐾, can be defined as the ratio of the pressure over the volumetric strain as the relative volume approaches unity: 𝑉 − 1 𝐾 = lim 𝑉→1 (22.27.7) ). ( The partial derivatives of 𝑊 lead to: LS-DYNA Theory Manual Material Models ∂𝑊 ∂𝐼1 𝜕𝑊 𝜕𝐼2 𝜕𝑊 𝜕𝐼3 = A, = B, = −2C𝐼3 −3 + 2D(𝐼3 − 1) = −2C𝜆−18 + 2D(𝜆6 − 1), (22.27.8) 𝑝 = = 𝜆3 {A𝜆2 + 2𝜆4B + 𝜆6[−2C𝜆−18 + 2D(𝜆6 − 1)]} 𝜆3 {A𝜆2 + 2𝜆4B − 2C𝜆−12 + 2D(𝜆12 − 𝜆6)}. In the limit as the stretch ratio approaches unity, the pressure must approach zero: lim 𝜆→1 𝑝 = 0. (22.27.9) Therefore, A + 2B − 2C = 0 and C = 0.5A + B. (22.27.10) To solve for D we note that: ) ( 𝑉 − 1 𝜆3 {A𝜆2 + 2𝜆4B − 2C𝜆−12 + 2D(𝜆12 − 𝜆6)} 𝜆3 − 1 A𝜆2 + 2𝜆4B − 2C𝜆−12 + 2D(𝜆12 − 𝜆6) 𝜆6 − 𝜆3 2A𝜆 + 8𝜆3B + 24C𝜆−13 + 2D(12𝜆11 − 6𝜆5) 6𝜆5 − 3𝜆2 (2A + 8B + 24C + 12D) (14A + 32B + 12D). 𝐾 = lim 𝑉→1 = lim λ→1 = 2lim λ→1 = 2lim λ→1 = = We therefore obtain: 14A + 32B + 12D = 𝐾 = ( 2𝐺(1 + 𝜐) 3(1 − 2𝜐) ) = 2(A + B)(1 + 𝜐) (1 − 2𝜐) . Solving for D we obtain the desired equation: D = A(5𝜐 − 2) + B(11𝜐 − 5) 2(1 − 2𝜐) . (22.27.11) (22.27.12) (22.27.13) Material Models LS-DYNA Theory Manual The invariants 𝐼1 − 𝐼3 are related to the right Cauchy-Green tensor C as 𝐼1 = 𝐶𝑖𝑖, 2 − 𝐼2 = 𝐶𝑖𝑖 𝐼3 = det(𝐶𝑖𝑗). 𝐶𝑖𝑗𝐶𝑖𝑗, (22.27.14) The second Piola-Kirchhoff stress tensor, S, is found by taking the partial derivative of the strain energy function with respect to the Green-Lagrange strain tensor, E. 𝑆𝑖𝑗 = ∂𝑊 ∂𝐸𝑖𝑗 = 2 ∂𝑊 ∂𝐶𝑖𝑗 = 2 [A ∂𝐼1 ∂𝐶𝑖𝑗 + B ∂𝐼2 ∂𝐶𝑖𝑗 + (2D(𝐼3 − 1) − 2C 2 ) 𝐼3 ∂I3 ∂𝐶𝑖𝑗 ]. (22.27.15) The derivatives of the invariants 𝐼1 − 𝐼3 are ∂𝐼1 ∂𝐶𝑖𝑗 ∂𝐼2 ∂𝐶𝑖𝑗 ∂𝐼3 ∂𝐶𝑖𝑗 = 𝛿𝑖𝑗, = 𝐼1𝛿𝑖𝑗 − 𝐶𝑖𝑗, = 𝐼3𝐶𝑖𝑗 −1. (22.27.16) Inserting Equation (22.27.16) into Equation (22.27.15) yields the following expression for the second Piola-Kirchhoff stress: 𝑆𝑖𝑗 = 2A𝛿𝑖𝑗 + 2B(𝐼1𝛿𝑖𝑗 − 𝐶𝑖𝑗) − 4C 2 𝐶𝑖𝑗 𝐼3 Equation (22.27.17) can be transformed into the Cauchy stress by using the push forward operation −1 + 4D(𝐼3 − 1)I3𝐶𝑖𝑗 (22.27.17) −1. 𝜎𝑖𝑗 = 𝐹𝑖𝑘𝑆𝑘𝑙𝐹𝑗𝑙. (22.27.18) where 𝐽 = det(𝐹𝑖𝑗). 22.27.1 Stress Update for Shell Elements As a basis for discussing the algorithmic tangent stiffness for shell elements in Section 19.27.3, the corresponding stress update as it is done in LS-DYNA is shortly recapitulated in this section. When dealing with shell elements, the stress (as well as constitutive matrix) is typically evaluated in corotational coordinates after which it is transformed back to the standard basis according to 22-94 (Material Models) 𝜎𝑖𝑗 = 𝑅𝑖𝑘𝑅𝑗𝑙𝜎̂𝑘𝑙. LS-DYNA Theory Manual Material Models Here 𝑅𝑖𝑗 is the rotation matrix containing the corotational basis vectors. The so- called corotated stress 𝜎̂𝑖𝑗 is evaluated using Equation 19.27.21 with the exception that the deformation gradient is expressed in the corotational coordinates, i.e., 𝜎̂𝑖𝑗 = 𝐹̂𝑖𝑘𝑆𝑘𝑙𝐹̂𝑗𝑙, (22.27.20) where 𝑆𝑖𝑗 is evaluated using Equation (22.27.17). The corotated deformation gradient is incrementally updated with the aid of a time increment Δ𝑡, the corotated velocity gradient 𝐿̂ 𝑖𝑗, and the angular velocity 𝛺̂𝑖𝑗 with which the embedded coordinate system is rotating. 𝐹̂𝑖𝑗 = (𝛿𝑖𝑘 + Δ𝑡𝐿̂ 𝑖𝑘 − Δ𝑡𝛺̂𝑖𝑘)𝐹̂𝑘𝑗. (22.27.21) The primary reason for taking a corotational approach is to facilitate the maintenance of a vanishing normal stress through the thickness of the shell, something that is achieved by adjusting the corresponding component of the corotated velocity gradient 𝐿̂ 33 accordingly. The problem can be stated as to determine 𝐿̂ 33 such that when updating the deformation gradient through Equation (22.27.21) and subsequently the stress through Equation (22.27.20), 𝜎̂33 = 0. To this end, it is assumed that 𝐿̂ 33 = 𝛼(𝐿̂ 11 + 𝐿̂ 22), (22.27.22) for some parameter α that is determined in the following three step procedure. In the (0) first two steps, 𝛼 = 0 and 𝛼 = −1, respectively, resulting in two trial normal stresses 𝜎̂33 (−1). Then it is assumed that the actual normal stress depends linearly on 𝛼, and 𝜎̂33 meaning that the latter can be determined from 0 = 𝜎33 (𝛼) = 𝜎33 (0) + 𝛼(𝜎33 (0) − 𝜎33 (−1)). In LS-DYNA, α is given by (0) 𝜎̂33 (−1) − 𝜎̂33 𝜎̂33 (0) ∣𝜎̂33 (−1) − 𝜎̂33 (0)∣ ≥ 10−4 − 1 otherwise 𝛼 = ⎧ { { { ⎨ { { { ⎩ (22.27.23) , (22.27.24) and the stresses are determined from this value of α. Finally, to make sure that the normal stress through the thickness vanishes, it is set to 0 (zero) before exiting the stress update routine. 22.27.2 Derivation of the Continuum Tangent Stiffness This section will describe the derivation of the continuum tangent stiffness for the Mooney-Rivlin material. For solid elements, the continuum tangent stiffness is Material Models LS-DYNA Theory Manual chosen in favor of an algorithmic (consistent) tangential modulus as the constitutive equation at hand is smooth and a consistent tangent modulus is not required for good convergence properties. For shell elements however, this stiffness must ideally be modified in order to account for the zero normal stress condition. This modification, and its consequences, are discussed in the next section. The continuum tangent modulus in the reference configuration is per definition, PK = 𝐸𝑖𝑗𝑘𝑙 ∂𝑆𝑖𝑗 ∂𝐸𝑘𝑙 = 2 ∂𝑆𝑖𝑗 ∂𝐶𝑘𝑙 . Splitting up the differentiation of Equation (22.27.17) we get ∂(𝐼1𝛿𝑖𝑗 − 𝐶𝑖𝑗) ∂𝐶𝑘𝑙 = 𝛿𝑘𝑙𝛿𝑖𝑗 − (𝛿𝑖𝑘𝛿𝑗𝑙 + 𝛿𝑖𝑙𝛿𝑗𝑘) −1) 𝜕 ( 1 2 𝐶𝑖𝑗 𝐼3 𝜕𝐶𝑘𝑙 = − 2 𝐶𝑘𝑙 𝐼3 −1𝐶𝑖𝑗 −1 − 2 (𝐶𝑘𝑗 2𝐼3 −1𝐶𝑖𝑙 −1 + 𝐶𝑙𝑗 −1𝐶𝑖𝑘 −1) 𝜕(𝐼3(𝐼3 − 1)𝐶𝑖𝑗 𝜕𝐶𝑘𝑙 −1) = 𝐼3(2𝐼3 − 1)𝐶𝑘𝑙 −1𝐶𝑖𝑗 −1 − 𝐼3(𝐼3 − 1)(𝐶𝑘𝑗 −1𝐶𝑖𝑙 −1 + 𝐶𝑙𝑗 −1𝐶𝑖𝑘 −1). (22.27.25) (22.27.26) (22.27.27) (22.27.28) Since LS-DYNA needs the tangential modulus for the Cauchy stress, it is a good idea to transform the terms in Equation (22.27.27) before summing them up. The push forward operation for the fourth-order tensor 𝐸𝑖𝑗𝑘𝑙 pk is TC = 𝐸𝑖𝑗𝑘𝑙 PK . 𝐹𝑖𝑎𝐹𝑗𝑏𝐹𝑘𝑐𝐹𝑙𝑑𝐸𝑎𝑏𝑐𝑑 (22.27.29) Since the right Cauchy-Green tensor is 𝐂 = 𝐅T𝐅 and the left Cauchy-Green tensor is 𝐛 = 𝐅T𝐅, and the determinant and trace of the both stretches are equal, the transformation is in practice carried out by interchanging −1 → 𝛿𝑖𝑗, 𝐶𝑖𝑗 𝛿𝑖𝑗 → 𝑏𝑖𝑗. (22.27.30) (22.27.31) The end result is then LS-DYNA Theory Manual Material Models 𝐽𝐸𝑖𝑗𝑘𝑙 TC = 4B [𝑏𝑘𝑙𝑏𝑖𝑗 − (𝑏𝑖𝑘𝑏𝑗𝑙 + 𝑏𝑖𝑙𝑏𝑗𝑘)] + 4C 2 [4𝛿𝑖𝑗𝛿𝑘𝑙 + (𝛿𝑘𝑗𝛿𝑖𝑙 + 𝛿𝑙𝑗𝛿𝑖𝑚)] + I3 (22.27.32) 8D𝐼3 [(2𝐼3 − 1)𝛿𝑖𝑗𝛿𝑘𝑙 − (𝐼3 − 1)(𝛿𝑘𝑗𝛿𝑖𝑙 + 𝛿𝑙𝑗𝛿𝑖𝑘)]. 22.27.3 The Algorithmic Tangent Stiffness for Shell Elements The corotated tangent stiffness matrix is given by Equation (22.27.32) with the exception that the left Cauchy-Green tensor and deformation gradient are given in corotational coordinates, i.e., 𝐽𝐸̂ TC = 4B [𝑏̂ 𝑖𝑗𝑘𝑙 𝑘𝑙𝑏̂ 𝑖𝑗 − (𝑏̂ 𝑖𝑘𝑏̂ 𝑗𝑙 + 𝑏̂ 𝑖𝑙𝑏̂ 𝑗𝑘)] + + 8D𝐼3 [(2𝐼3 − 1)𝛿𝑖𝑗𝛿𝑘𝑙 − 4C 2 [4𝛿𝑖𝑗𝛿𝑘𝑙 + (𝛿𝑘𝑗𝛿𝑖𝑙 + 𝛿𝑙𝑗𝛿𝑖𝑚)] 𝐼3 (𝐼3 − 1)(𝛿𝑘𝑗𝛿𝑖𝑙 + 𝛿𝑙𝑗𝛿𝑖𝑘)]. (22.27.33) Using this exact expression for the tangent stiffness matrix in the context of shell elements is not adequate since it does not take into account that the normal stress is zero and it must be modified appropriately. To this end, we assume that the tangent moduli in Equation (22.27.33) relates the corotated rate-of-deformation tensor 𝐷̂ 𝑖𝑗 to the •, corotated rate of stress 𝜎̂𝑖𝑗 • = 𝐸̂ 𝜎̂𝑖𝑗 TC𝐷̂ 𝑘𝑙. 𝑖𝑗𝑘𝑙 (22.27.34) Even though this is not completely true, we believe that attempting a more thorough treatment would hardly be worth the effort. The objective can now be stated as to find a modified tangent stiffness matrix 𝐸̂ TCalg such that ijkl •alg = 𝐸̂ 𝜎̂𝑖𝑗 TCalg𝐷̂ 𝑘𝑙, 𝑖𝑗𝑘𝑙 (22.27.35) alg is the stress as it is evaluated in LS-DYNA. The stress update, described in where 𝜎̂𝑖𝑗 Section 19.27.1, is performed in a rather ad hoc way which probably makes the stated objective unachievable. Still we attempt to extract relevant information from it that enables us to come somewhat close. An example of a modification of this tangent moduli is due to Hughes and Liu [1981] and given by 𝐸̂ TCalg = 𝐸̂ 𝑖𝑗𝑘𝑙 TC − 𝑖𝑗𝑘𝑙 TC 33𝑘𝑙 TC 𝐸̂ 𝐸̂𝑖𝑗33 𝐸̂ TC 3333 . (22.27.36) Material Models LS-DYNA Theory Manual This matrix is derived by eliminating the thickness strain 𝐷̂ 33 from the equation • = 0 in Equation (22.27.35) as an unknown. This modification is unfortunately not 𝜎̂33 consistent with how the stresses are updated in LS-DYNA. When consulting Section 19.27.1, it is suggested that 𝐷̂ 33 instead can be eliminated from 𝐷̂ 33 = 𝛼(𝐷̂ 11 + 𝐷̂ 22), (22.27.37) using the α determined from the stress update. Unfortunately, by the time when the tangent stiffness matrix is calculated, the exact value of α is not known. From experimental observations however, we have found that α is seldom far from being equal to −1. The fact that α = −1 represents incompressibility strengthen this TC except hypothesis. This leads to a modified tangent stiffness 𝐸̂ 𝑖𝑗𝑘𝑙 for the following modifications, TCalg that is equal to 𝐸̂ 𝑖𝑗𝑘𝑙 𝐸̂ 𝐸̂ TCalg = 𝐸̂𝑖𝑖𝑗𝑗 𝑖𝑖𝑗𝑗 TCalg = 𝐸̂ 33𝑖𝑗 TC − 𝐸̂33𝑗𝑗 TC − 𝐸̂𝑖𝑖33 TCalg = 0, 𝑖 ≠ 𝑗. 𝑖𝑗33 TC , TC + 𝐸̂3333 (22.27.38) To preclude the obvious singularity, a small positive value is assigned to 𝐸̂ TCalg, 3333 𝐸̂ TCalg = 10−4(∣𝐸̂ 3333 TCalg∣ + ∣𝐸̂ 1111 TCalg∣). 2222 (22.27.39) As with the Hughes-Liu modification, this modification preserves symmetry and positive definiteness of the tangent moduli, which together with the stress update “consistency” makes it intuitively attractive. LS-DYNA Theory Manual Material Models 22.28 Material Model 28: Resultant Plasticity This plasticity model, based on resultants as illustrated in Figure 22.28.1, is very cost effective but not as accurate as through-thickness integration. This model is available only with the C0 triangular, Belytschko-Tsay shell, and the Belytschko beam element since these elements, unlike the Hughes-Liu elements, lend themselves very cleanly to a resultant formulation. (a) Membrane (b) Bending Figure 22.28.1. Full section yield using resultant plasticity. In applying this model to shell elements the resultants are updated incrementally using the midplane strains 𝜀m and curvatures 𝜅: Δ𝑛 = Δ𝑡𝐶𝜀m Δ𝑚 = Δ𝑡 ℎ3 12 𝐶𝜅, (22.28.1) (22.28.2) where the plane stress constitutive matrix is given in terms of Young’s Modulus 𝐸 and Poisson’s ratio 𝜈 as: 𝑚̅̅̅̅̅ = 𝑚𝑥𝑥 2 − 𝑚𝑥𝑥𝑚𝑦𝑦 + 𝑚𝑦𝑦 2 . 2 + 3𝑚𝑥𝑦 Defining 𝑛̅ = 𝑛𝑥𝑥 2 − 𝑛𝑥𝑥𝑛𝑦𝑦 + 𝑛𝑦𝑦 2 , 2 + 3𝑛𝑥𝑦 𝑚̅̅̅̅̅ = 𝑚𝑥𝑥 2 − 𝑚𝑥𝑥𝑚𝑦𝑦 + 𝑚𝑦𝑦 2 , 2 + 3𝑚𝑥𝑦 𝑚̅̅̅̅̅𝑛̅ = 𝑚𝑥𝑥𝑛𝑥𝑥 − 𝑚𝑥𝑥𝑛𝑦𝑦 − 𝑛𝑥𝑥𝑚𝑦𝑦 + 𝑚𝑦𝑛𝑦 + 3𝑚𝑥𝑦𝑛𝑥𝑦, the Ilyushin yield function becomes 𝑓 (𝑚, 𝑛) = 𝑛̅ + 4|𝑚̅̅̅̅̅𝑛̅| ℎ√3 + 16𝑚̅̅̅̅̅ ℎ2 ≤ 𝑛y 2 = ℎ2𝜎y 2. (22.28.3) (22.28.4) (22.28.5) (22.28.6) (22.28.7) Material Models LS-DYNA Theory Manual In our implementation we update the resultants elastically and check to see if the yield condition is violated: If so, the resultants are scaled by the factor 𝛼: 2. 𝑓 (𝑚, 𝑛) > 𝑛y 𝛼 = √ 𝑛y . 𝑓 (𝑚, 𝑛) We update the yield stress incrementally: (22.28.8) (22.28.9) 𝑛 + 𝐸PΔ𝜀plastic where 𝐸P is the plastic hardening modulus which in incremental plastic strain is approximated by 𝑛+1 = 𝜎y 𝜎y (22.28.10) eff , eff Δ𝜀plastic = √𝑓 (𝑚, 𝑛) − 𝑛y ℎ(3𝐺 + 𝐸𝑝) . (22.28.11) Kennedy, et. al., report that this model predicts results that may be too stiff; users of this model should proceed cautiously. In applying this material model to the Belytschko beam, the flow rule changes to 𝑓 (𝑚, 𝑛) = 𝑓 ̂ 2 + 2𝐴 4𝑚̂𝑦 3𝐼𝑦𝑦 + 2𝐴 4𝑚̂𝑧 3𝐼𝑧𝑧 ≤ 𝑛y 2, 2 = 𝐴2𝜎y (22.28.12) have been updated elastically according to Equations (4.16)-(4.18). The yield condition is checked with Equation (22.28.8), and if it is violated, the resultants are scaled as described above. This model is frequently applied to beams with non-rectangular cross sections. The accuracy of the results obtained should be viewed with some healthy suspicion. No work hardening is available with this model. LS-DYNA Theory Manual Material Models 22.29 Material Model 29: FORCE LIMITED Resultant Formulation This material model is available for the Belytschko beam element only. Plastic hinges form at the ends of the beam when the moment reaches the plastic moment. The moment-versus-rotation relationship is specified by the user in the form of a load curve and scale factor. The point pairs of the load curve are (plastic rotation in radians, plastic moment). Both quantities should be positive for all points, with the first point pair being (zero, initial plastic moment). Within this constraint any form of characteristic may be used including flat or falling curves. Different load curves and scale factors may be specified at each node and about each of the local s and t axes. Axial collapse occurs when the compressive axial load reaches the collapse load. The collapse load-versus-collapse deflection is specified in the form of a load curve. The points of the load curve are (true strain, collapse force). Both quantities should be entered as positive for all points, and will be interpreted as compressive i.e., collapse does not occur in tension. The first point should be the pair (zero, initial collapse load). The collapse load may vary with end moment and with deflection. In this case, several load-deflection curves are defined, each corresponding to a different end moment. Each load curve should have the same number of point pairs and the same deflection values. The end moment is defined as the average of the absolute moments at each end of the beam, and is always positive. It is not possible to make the plastic moment vary with axial load. A co-rotational technique and moment-curvature relations are used to compute the internal forces. The co-rotational technique is treated in Section 4 in and will not be treated here as we will focus solely on the internal force update and computing the tangent stiffness. For this we use the notation Material Models LS-DYNA Theory Manual M8 M7 M6 M5 M4 M3 M2 M1M1 Strain (or change in length, see AOPT) Figure 22.29.1. The force magnitude is limited by the applied end moment. For an intermediate value of the end moment, LS-DYNA interpolates between the curves to determine the allowable force. 𝐸 = Young′smodulus 𝐺 = Shear modulus 𝐴 = Cross sectional area 𝐴s = Effective area in shear 𝑙𝑛 = Reference length of beam 𝑙𝑛+1 = Current length of beam 𝐼𝑦𝑦 = Second moment of inertia about 𝑦 𝐼𝑧𝑧 = Second moment of inertia about 𝑧 𝐽 = Polar moment of inertia 𝑒𝑖 = 𝑖th local base vector in the current configuration 𝑦𝐼 = nodal vector in y direction at node I in the current configuration 𝑧𝐼 = nodal vector in z direction at node I in the current configuration (22.29.1) LS-DYNA Theory Manual Material Models We emphasize that the local 𝑦 and 𝑧 base vectors in the reference configuration always coincide with the corresponding nodal vectors. The nodal vectors in the current configuration are updated using the Hughes-Winget formula while the base vectors are computed from the current geometry of the element and the current nodal vectors. 22.29.1 Internal Forces Elastic Update In the local system for a beam connected by nodes I and J, the axial force is updated as where el = 𝐟a 𝐟a n + Ka el𝛅, 𝐾a 𝐸𝐴 el = 𝑙𝑛 , 𝛿 = 𝑙𝑛+1 − 𝑙𝑛. The torsional moment is updated as 𝑚t el = 𝑚t n + 𝐾t el𝜃t, where el = 𝐾t 𝜃t = 𝐺𝐽 𝑙𝑛 , T(𝐲I × 𝐲J + 𝐳I × 𝐳J). 𝐞1 The bending moments are updated as n + 𝐀𝑦 el = 𝐦𝑦 𝐦𝑦 el𝛉𝑦 𝐦𝑧 el = 𝐦𝑧 n + 𝐀𝑧 el𝛉𝑧, where el = 𝐀∗ 1 + 𝜑∗ 𝐸𝐼∗∗ 𝑙n [ 4 + 𝜑∗ 2 − 𝜑∗ 2 − 𝜑∗ 4 + 𝜑∗ ] 𝜑∗ = 12𝐸𝐼∗∗ 𝐺𝐴slnln T = −𝐞3 𝛉y T(𝐲I × 𝐳I 𝐲J × 𝐳J) T = 𝐞2 𝛉z T(𝐲I × 𝐳I 𝐲J × 𝐳J). (22.29.2) (22.29.3) (22.29.4) (22.29.5) (22.29.6) (22.29.7) (22.29.8) (22.29.9) (22.29.10) (22.29.11) In the following we refer to 𝐀∗ el as the (elastic) moment-rotation matrix. Material Models Plastic Correction LS-DYNA Theory Manual After the elastic update the state of force is checked for yielding as follows. As a preliminary note we emphasize that whenever yielding does not occur the elastic stiffnesses and forces are taken as the new stiffnesses and forces. Y(𝜃𝑖𝐼 The yield moments in direction 𝑖 at node 𝐼 as functions of plastic rotations are P). This function is given by the user but also depends on whether a denoted 𝑚𝑖𝐼 plastic hinge has been created. The theory for plastic hinges is given in the LS-DYNA Keyword User’s Manual [Hallquist 2003] and is not treated here. Whenever the elastic moment exceeds the plastic moment, the plastic rotations are updated as P(𝑛+1) = 𝜃𝑖𝐼 𝜃𝑖𝐼 P(𝑛) + ∣𝑚𝑖𝐼 el∣ − 𝑚𝑖𝐼 max (0.001, 𝐴𝑖(𝐼𝐼) el + , ∂𝑚𝑖𝐼 P ) ∂𝜃𝑖𝐼 and the moment is reduced to the yield moment 𝑚𝑖𝐼 𝑛+1 = 𝑚𝑖𝐼 Y(𝜃𝑖𝐼 P(𝑛+1))sgn(𝑚𝑖𝐼 el). (22.29.12) (22.29.13) The corresponding diagonal component in the moment-rotation matrix is reduced as 𝑛+1 = 𝐴𝑖(𝐼𝐼) 𝐴𝑖(II) el 1 − 𝛼 ⎜⎜⎜⎜⎜⎜⎜⎜⎛ ⎝ el 𝐴𝑖(𝐼𝐼) max (0.001, 𝐴𝑖(𝐼𝐼) el + , ⎟⎟⎟⎟⎟⎟⎟⎟⎞ ⎠ ∂𝑚𝑖𝐼 P ) ∂𝜃𝑖𝐼 (22.29.14) where α ≤ 1 is a parameter chosen such that the moment-rotation matrix remains positive definite. The yield moment in torsion is given by 𝑚t P) and is provided by the user. If the elastic torsional moment exceeds this value, the plastic torsional rotation is updated as Y(𝜃t P(𝑛+1) = 𝜃t 𝜃t P(𝑛) + ∣𝑚t el∣ − 𝑚t max (0.001, 𝐾t el + , ∂𝑚t P ) ∂𝜃t and the moment is reduced to the yield moment 𝑚t 𝑛+1 = 𝑚t Y(𝜃t P(𝑛+1))sgn(𝑚t el). (22.29.15) (22.29.16) The torsional stiffness is modified as LS-DYNA Theory Manual Material Models 𝐾t el n+1 = 𝐾t 1 − α ⎜⎜⎜⎜⎜⎜⎜⎜⎛ ⎝ el 𝐾t ⎟⎟⎟⎟⎟⎟⎟⎟⎞ ∂𝑚t ∂𝜃t P ⎠ el + 𝐾t , (22.29.17) where again α ≤ 1 is chosen so that the stiffness is positive. Axial collapse is modeled by limiting the axial force by 𝑓a Y(𝜀, 𝑚), i.e., a function of the axial strains and the magnitude of bending moments. If the axial elastic force exceeds this value it is reduced to yield 𝑛+1 = 𝑓a 𝑓a and the axial stiffness is given by Y(𝜀𝑛+1, 𝑚𝑛+1)sgn(𝑓a el), 𝐾a el, 𝑛+1 = max (0.05𝐾a ∂𝑓a ∂𝜀 ). (22.29.18) (22.29.19) We neglect the influence of change in bending moments when computing this parameter. Damping Damping is introduced by adding a viscous term to the internal force on the form 𝐟v = 𝐃 𝑑𝑡 ⎤ ⎡ 𝜃t ⎥ ⎢ , ⎥ ⎢ 𝜃𝑦 ⎥ ⎢ 𝜃𝑧⎦ ⎣ 𝐃 = 𝛾 el ⎡𝐾a ⎢ ⎢ ⎢ ⎢ ⎣ el 𝐾t el 𝐴𝑦 ⎤ ⎥ ⎥ , ⎥ ⎥ el⎦ 𝐴𝑧 (22.29.20) (22.29.21) where γ is a damping parameter. Transformation The internal force vector in the global system is obtained through the transformation where 𝑛+1 = 𝐒𝐟l 𝐟g 𝑛+1, (22.29.22) Material Models LS-DYNA Theory Manual −𝑒3/𝑙𝑛+1 −𝑒3/𝑙𝑛+1 𝐒 = −𝑒1 ⎡ ⎢ ⎢ 𝑒1 ⎢ ⎣ −𝑒1 𝑒1 𝑒2 𝑒3/𝑙𝑛+1 𝑒2/𝑙𝑛+1 𝑒3 𝑒3/𝑙𝑛+1 −𝑒2/𝑙𝑛+1 −𝑒2/𝑙𝑛+1 𝑒2/𝑙𝑛+1 𝑒2 𝑒3 𝑛+1 = 𝐟l 𝑛+1 𝑛+1 fa ⎡ ⎢ 𝑚t ⎢ ⎢ 𝑚y ⎢ 𝑚z ⎣ ⎤ ⎥ ⎥ ⎥ ⎥ 𝑛+1⎦ 𝑛+1 . ⎤ ⎥ , ⎥ ⎥ ⎦ (22.29.23) (22.29.24) 22.29.2 Tangent Stiffness Derivation The tangent stiffness is derived from taking the variation of the internal force δ𝐟g 𝑛+1 = δ𝐒𝐟l 𝑛+1 + 𝐒δ𝐟l 𝑛+1, which can be written where 𝑛+1 = 𝐊geoδ𝐮 + 𝐊matδ𝐮, δ𝐟g δ𝐮 = [δx𝐼 δω𝐼 δx𝐽 δω𝐽 T] . (22.29.25) (22.29.26) (22.29.27) There are two contributions to the tangent stiffness, one geometrical and one material contribution. The geometrical contribution is given (approximately) by 𝐊geo = 𝐑(𝐟l 𝑛+1 ⊗ 𝐈)𝐖 − l𝑛+1l𝑛+1 𝐓𝐟l 𝑛+1𝐋, where 𝐑 = 𝑅1 ⎡ ⎢ ⎢ −𝑅1 ⎢ ⎣ 𝑅1 −𝑅1 𝑅3/𝑙𝑛+1 −𝑅2 𝑅3/𝑙𝑛+1 −𝑅2/𝑙𝑛+1 −𝑅2/𝑙𝑛+1 −𝑅3 𝑅2/𝑙𝑛+1 𝑅2/𝑙𝑛+1 −𝑅3 −𝑅2 −𝑅3/𝑙𝑛+1 −𝑅3/𝑙𝑛+1 𝐖 = [−𝑅1/𝑙𝑛+1 𝐞1𝐞1 T/2 𝑅1/𝑙𝑛+1 𝐞1𝐞1 T/2], 𝐓 = ⎡ ⎢ ⎢ ⎣ 𝑒2 0 −𝑒3 −𝑒3 𝑒2 ⎤ ⎥ , ⎥ 𝑒3 𝑒3 −𝑒2 −𝑒2 0 ⎦ 𝐋 = [−𝐞1 𝐞1 0], ⎤ ⎥ , ⎥ ⎥ ⎦ (22.29.28) (22.29.29) (22.29.30) (22.29.31) (22.29.32) and 𝐈 is the 3 by 3 identity matrix. We use ⊗ as the outer matrix product and define LS-DYNA Theory Manual Material Models Riv = 𝐞i × 𝐯. The material contribution can be written as 𝐊mat = 𝐒𝐊𝐒T, where 𝐊 = 𝑛+1 𝐾a ⎡ ⎢ ⎢ ⎢ ⎢ ⎣ 𝑛+1 𝐾t 𝑛+1 𝐴y ⎤ ⎥ ⎥ ⎥ ⎥ 𝑛+1⎦ 𝐴z + Δ𝑡 𝐃. (22.29.33) (22.29.34) (22.29.35) Material Models LS-DYNA Theory Manual 22.30 Material Model 30: Closed-Form Update Shell Plasticity This section presents the mathematical details of the shape memory alloy material in LS-DYNA. The description closely follows the one of Auricchio and Taylor [1997] with appropriate modifications for this particular implementation. 22.30.1 Mathematical Description of the Material Model The Kirchhoff stress 𝛕 in the shape memory alloy can be written where 𝐢 is the second order identity tensor and 𝛕 = 𝑝𝐢 + 𝐭, 𝑝 = 𝐾(𝜃 − 3α𝜉S𝜀L), 𝐭 = 2𝐺(𝐞 − 𝜉S𝜀L𝐧). (22.30.1) (22.30.2) (22.30.3) Here 𝐾 and 𝐺 are bulk and shear modulii, 𝜃 and e are volumetric and shear logarithmic strains and 𝛼 and 𝜀L are constant material parameters. There is an option to define the bulk and shear modulii as functions of the martensite fraction according to 𝐾 = 𝐾A + 𝜉S(𝐾S − 𝐾A), 𝐺 = 𝐺A + 𝜉S(𝐺S − 𝐺A), (22.30.4) in case the stiffness of the martensite differs from that of the austenite. Furthermore, the unit vector 𝐧 is defined as and a loading function is introduced as 𝐧 = 𝐞/(‖𝐞‖ + 10−12), where 𝐹 = 2𝐺‖𝐞‖ + 3𝛼𝐾𝜃 − 𝛽𝜉S, 𝛽 = (2𝐺 + 9𝛼2𝐾)𝜀L. (22.30.5) (22.30.6) (22.30.7) For the evolution of the martensite fraction 𝜉S in the material, the following rule is adopted AS > 0 𝐹 − 𝑅s 𝐹̇ > 0 𝜉S < 1 }⎫ }⎬ ⎭ ⇒ 𝜉 ̇ S = −(1 − 𝜉S) 𝐹̇ 𝐹 − 𝑅f AS (22.30.8) LS-DYNA Theory Manual Material Models SA < 0 𝐹 − 𝑅s 𝐹̇ < 0 𝜉S > 0 }⎫ }⎬ ⎭ ⇒ 𝜉 ̇ S = 𝜉S 𝐹̇ 𝐹 − 𝑅f SA . (22.30.9) AS, 𝑅s stress is finally obtained as Here 𝑅s AS, 𝑅f SA and 𝑅f SA are constant material parameters. The Cauchy 𝛔 = , (22.30.10) where 𝐽 is the Jacobian of the deformation. 22.30.2 Algorithmic Stress Update For the stress update we assume that the martensite fraction 𝜉S 𝑛 and the value of the loading function F𝑛 is known from time 𝑡𝑛 and the deformation gradient at time 𝑡𝑛+1, F, is known. We form the left Cauchy-Green tensor as 𝐁 = 𝐅𝐅Twhich is diagonalized to obtain the principal values and directions 𝚲 = diag(λi) and 𝐐. The volumetric and principal shear logarithmic strains are given by 𝜃 = log(𝐽) , ⎜⎜⎜⎛𝜆𝑖 ⎟⎟⎟⎞ 3⎠ ⎝ 𝑒𝑖 = log , (22.30.11) where (22.30.12) 𝐽 = 𝜆1𝜆2𝜆3. 𝑛, a value is the total Jacobian of the deformation. Using Equation (22.30.6) with 𝜉S = 𝜉S 𝐹trial of the loading function can be computed. The discrete counterpart of Equation (22.30.8) becomes 𝐹trial − 𝑅s 𝐹trial − 𝐹n > 0 n < 1 𝜉S AS > 0 ⇒ Δ𝜉S ⎫ } ⎬ } ⎭ (22.30.13) = −(1 − 𝜉S 𝑛 − Δ𝜉S) 𝐹trial − 𝛽Δ𝜉S − min(max(𝐹𝑛, 𝑅s AS), 𝑅f AS) 𝐹trial − 𝛽Δ𝜉S − 𝑅f AS SA < 0 𝐹trial − 𝑅s 𝐹trial − 𝐹n < 0 n > 0 𝜉S ⎫ } ⎬ } ⎭ ⇒ Δ𝜉S = (𝜉S 𝑛 + Δ𝜉𝑆) 𝐹trial − 𝛽Δ𝜉S − min(max(𝐹n, 𝑅f SA 𝐹trial − 𝛽Δ𝜉S − 𝑅f SA) , 𝑅s SA) . (22.30.14) If none of the two conditions to the left are satisfied, set 𝜉S 𝑛, 𝐹𝑛+1 = 𝐹trial and compute the stress 𝜎 𝑛+1 using Equations (22.30.1), (22.30.2), (22.30.5), (22.30.10) and 𝑛. When phase transformation occurs according to a condition to the left, the 𝜉S = 𝜉S 𝑛+1 = 𝜉S Material Models LS-DYNA Theory Manual corresponding equation to the right is solved for Δ𝜉S. If the bulk and shear modulii are constant this is an easy task. Otherwise 𝐹trial as well as 𝛽 depends on this parameter and makes things a bit more tricky. We have that 𝐹trial = 𝐹n trial (1 + 𝛽 = 𝛽n (1 + 𝐸S − 𝐸A 𝐸n 𝐸S − 𝐸A 𝐸n Δ𝜉S), Δ𝜉S) , (22.30.15) where 𝐸S and 𝐸A are Young’s modulii for martensite and austenite, respectively. The subscript 𝑛 is introduced for constant quantities evaluated at time 𝑡𝑛. To simplify the upcoming expressions, these relations are written trial + Δ𝐹trialΔ𝜉S, (22.30.16) 𝐹trial = 𝐹n 𝛽 = 𝛽n + Δ𝛽Δ𝜉S. Inserting these expressions into Equation (19.30.7) results in 𝑓 (Δ𝜉S) = Δ𝛽(1 − 𝜉S 𝑛 − 𝐹𝑛 𝑛)(𝐹̃AS (1 − 𝜉S 𝑛)Δ𝜉S trial) = 0. 2 + (𝑅f AS − 𝐹̃AS 𝑛 + (𝛽n − Δ𝐹trial)(1 − 𝜉S 𝑛)) Δ𝜉S + and 𝑓 (Δ𝜉S) = Δ𝛽𝜉S 𝑛 − 𝐹𝑛 𝑛(𝐹̃SA 𝜉S 𝑛Δ𝜉S trial) = 0. 2 + (𝐹̃SA 𝑛 − 𝑅f SA + (𝛽𝑛 − Δ𝐹trial)𝜉S 𝑛)Δ𝜉S + respectively, where we have for simplicity set 𝑛 = min(max(𝐹𝑛, 𝑅s 𝐹̃AS 𝑛 = min(max(𝐹𝑛, 𝑅f 𝐹̃SA AS) , 𝑅f SA), 𝑅s AS) , SA). (22.30.17) (22.30.18) (22.30.19) The solutions to these equations are approximated with two Newton iterations 𝑛 + Δ𝜉S)) and compute starting in the point Δ𝜉S = 0. Now set 𝜉S 𝜎 𝑛+1 and 𝐹𝑛+1 according to Equations (22.30.1), (22.30.2), (22.30.5), (22.30.6), (22.30.10) and 𝜉S = 𝜉S 𝑛+1 = min(1, max(0, 𝜉S 𝑛+1. 22.30.3 Tangent Stiffness Matrix An algorithmic tangent stiffness matrix relating a change in true strain to a corresponding change in Kirchhoff stress is derived in the following. Taking the variation of Equation (22.30.2) results in δ𝑝 = 𝐾(δ𝜃 − 3𝛼δ𝜉S𝜀L) + δ𝐾(𝜃 − 3𝛼𝜉S𝜀L), δ𝐭 = 2𝐺(δ𝐞 − δ𝜉S𝜀L𝐧 − 𝜉S𝜀Lδ𝐧) + 2δ𝐺(𝐞 − 𝜉S𝜀L𝐧). (22.30.20) (22.30.21) LS-DYNA Theory Manual Material Models The variation of the unit vector in Equation (22.30.5) can be written δ𝐧 = ‖𝐞‖ + 10−12 (𝐈 − 𝐧 ⊗ 𝐧)δ𝐞, (22.30.22) where 𝐈 is the fourth order identity tensor. For the variation of martensite fraction we introduce the indicator parameters 𝐻AS and 𝐻SA that should give information of the probability of phase transformation occurring in the next stress update. Set initially 𝐻AS = 𝐻SA = 0 and change them according to AS > 0 𝐹trial − 𝑅s ⎫ } 𝐹trial − 𝐹𝑛 > 0 ⎬ } 𝑛 + Δ𝜉S ≤ 1 ⎭ 𝜉S SA < 0 𝐹trial − 𝑅s ⎫ } 𝐹trial − 𝐹𝑛 < 0 ⎬ } 𝑛 + Δ𝜉S ≥ 0 ⎭ 𝜉S ⇒ 𝐻AS = 1, (22.30.23) ⇒ 𝐻SA = 1, (22.30.24) using the quantities computed in the previous stress update. For the variation of the martensite fraction we take variations of Equations (22.30.17) and (22.30.18) with which results in trial = 2𝐺𝐧: δ𝐞 + 3𝛼𝐾δ𝜃, δ𝐹n δ𝜉S = γ(2𝐺𝐧: δ𝐞 + 3𝛼𝐾δ𝜃), where 𝛾 = 𝑛)𝐻AS (1 − 𝜉S 𝑛 + (𝛽𝑛 − Δ𝐹𝑛 AS AS − 𝐹̃ 𝑅f 𝑛) trial)(1 − 𝜉S 𝐹̃ 𝑛 − 𝑅f SA + 𝑛𝐻SA 𝜉S SA + (𝛽𝑛 − Δ𝐹𝑛 trial)𝜉S (22.30.25) (22.30.26) . (22.30.27) As can be seen, we use the value of 𝛾 obtained in the previous stress update since this is easier to implement and will probably give a good indication of the current value of this parameter. The variation of the material parameters 𝐾 and 𝐺 results in δK = (𝐾S − 𝐾A)δ𝜉S, δG = (𝐺S − 𝐺A)δ𝜉S, and, finally, using the identities 𝐧: δ𝐞 = 𝐧: δ𝛆, δ𝜃 = 𝐢: δ𝛆, δ𝛕 = 𝐢δ𝑝 + δ𝐭, results in (22.30.28) (22.30.29) (22.30.30) (22.30.31) Material Models LS-DYNA Theory Manual δ𝛕 = {2𝐺 (1 − 𝜉S𝜀L ‖𝐞‖ + 10−12) 𝐈dev + 𝐾[1 − 9𝛼2𝐾𝛾𝜀L + 3𝛼𝛾(𝐾S − 𝐾A)(𝜃 − 3𝛼𝜉S𝜀L)]𝐢 ⊗ 𝐢 + 2γ𝐺(𝐾S − 𝐾A)(𝜃 − 3𝛼𝜉S𝜀L)𝐢 ⊗ 𝐧 + 6𝛾𝛼𝐾(𝐺S − 𝐺A)(‖𝐞‖ − 𝜉S𝜀L)𝐧 ⊗ 𝐢 (22.30.32) + 2𝐺 [ 𝜉S𝜀L ‖𝐞‖ + 10−12 − 2𝐺𝛾𝜀L + 2𝛾(𝐺S − 𝐺A)(‖𝐞‖ − 𝜉S𝜀L)] 𝐧 ⊗ 𝐧 − 6𝐾𝐺𝛼𝛾𝜀L(𝐢 ⊗ 𝐧 + 𝐧 ⊗ 𝐢)} δ𝜀. where 𝐈dev is the fourth order deviatoric identity tensor. In general this tangent is not symmetric because of the terms on the second line in the expression above. We simply implementation. use a symmetrization of the tangent stiffness above Furthermore, we transform the tangent to a tangent closer related to the one that should be used in the LS-DYNA implementation, in the 𝐂 = 𝐽−1 {2𝐺 (1 − 𝜉S𝜀L ‖𝐞‖ + 10−12) 𝐈dev + 𝐾[1 − 9𝛼2𝐾𝛾𝜀L + 3𝛼𝛾(𝐾S − 𝐾A)(𝜃 − 3𝛼𝜉S𝜀L)]𝐢 ⊗ 𝐢 + 3𝛾𝛼𝐾(𝐺S − 𝐺A)(‖𝐞‖ − 𝜉S𝜀L) − 6𝐾𝐺𝛼𝛾𝜀L))(𝐢 ⊗ 𝐧 + 𝐧 ⊗ 𝐢) (22.30.33) + 2G [ 𝜉S𝜀L ‖𝐞‖ + 10−12 − 2𝐺𝛾𝜀L + 2𝛾(𝐺S − 𝐺A)(‖𝐞‖ − 𝜉S𝜀L)] 𝐧 ⊗ 𝐧} δ𝜀. LS-DYNA Theory Manual Material Models 22.31 Material Model 31: Slightly Compressible Rubber Model This model implements a modified form of the hyperelastic constitutive law first described in [Kenchington 1988]. The strain energy functional, 𝑈, is defined in terms of the input constants as: 𝑈 = C100𝐼1 + C200𝐼1 C210𝐼1 2𝐼2 + C010𝐼2 + C020𝐼2 2 + C300𝐼1 3 + C400𝐼1 2 + 𝑓 (𝐽), 4 + C110𝐼1𝐼2 + (22.31.1) where the strain invariants can be expressed in terms of the deformation gradient matrix, 𝐹𝑖𝑗, and the Green-St. Venant strain tensor, 𝐸𝑖𝑗: 𝐽 = ∣𝐹𝑖𝑗∣ 𝐼1 = 𝐸𝑖𝑖 𝐼2 = 𝑖𝑗 𝐸𝑝𝑖𝐸𝑞𝑗. 𝛿𝑝𝑞 2! (22.31.2) The derivative of 𝑈 with respect to a component of strain gives the correspond- ing component of stress 𝑆𝑖𝑗 = ∂𝑈 ∂𝐸𝑖𝑗 , (22.31.3) where, 𝑆𝑖𝑗, is the second Piola-Kirchhoff stress tensor which is transformed into the Cauchy stress tensor: 𝜎𝑖𝑗 = 𝜌0 𝜕𝑥𝑖 𝜕𝑋𝑘 𝜕𝑥𝑗 𝜕𝑋𝑙 𝑆𝑘𝑙, (22.31.4) where 𝜌0 and 𝜌 are the initial and current density, respectively. Material Models LS-DYNA Theory Manual 22.32 Material Model 32: Laminated Glass Model This model is available for modeling safety glass. Safety glass is a layered material of glass bonded to a polymer material which can undergo large strains. The glass layers are modeled by isotropic hardening plasticity with failure based on exceeding a specified level of plastic strain. Glass is quite brittle and cannot withstand large strains before failing. Plastic strain was chosen for failure since it increases monotonically and, therefore, is insensitive to spurious numerical noise in the solution. The material to which the glass is bonded is assumed to stretch plastically without failure. The user defined integration rule option must be used with this material. The user defined rule specifies the thickness of the layers making up the safety glass. Each integration point is flagged with a zero if the layer is glass and with a one if the layer is polymer. An iterative plane stress plasticity algorithm is used to enforce the plane stress condition. LS-DYNA Theory Manual Material Models 22.33 Material Model 33: Barlat’s Anisotropic Plasticity Model This model was developed by Barlat, Lege, and Brem [1991] for modeling material behavior in forming processes. The finite element implementation of this model is described in detail by Chung and Shah [1992] and is used here. The yield function 𝛷 is defined as 𝛷 = |𝑆1 − 𝑆2|𝑚 + |𝑆2 − 𝑆3|𝑚 + |𝑆3 − 𝑆1|𝑚 = 2𝑚, (22.33.1) where 𝜎̅̅̅̅̅ is the effective stress, and 𝑆𝑖 for 𝑖 = 1, 2, 3 are the principal values of the symmetric matrix 𝑆𝛼𝛽, 𝑆𝑥𝑥 = 𝑆𝑦𝑦 = [𝑐(𝜎𝑥𝑥 − 𝜎𝑦𝑦) − 𝑏(𝜎𝑧𝑧 − 𝜎𝑥𝑥)] [𝑎(𝜎𝑦𝑦 − 𝜎𝑧𝑧) − 𝑐(𝜎𝑥𝑥 − 𝜎𝑦𝑦)] [𝑏(𝜎𝑧𝑧 − 𝜎𝑥𝑥) − 𝑎(𝜎𝑦𝑦 − 𝜎𝑧𝑧)] 𝑆𝑧𝑧 = 𝑆𝑦𝑧 = 𝑓 𝜎𝑦𝑧 𝑆𝑧𝑥 = 𝑔𝜎𝑧𝑥 𝑆𝑥𝑦 = ℎ𝜎𝑥𝑦. (22.33.2) The material constants 𝑎, 𝑏, 𝑐, 𝑓 , 𝑔 and ℎ represent anisotropic properties. When 𝑎 = 𝑏 = 𝑐 = 𝑓 = 𝑔 = ℎ = 1, the material is isotropic and the yield surface reduces to the Tresca yield surface for 𝑚 = 1 and von Mises yield surface for 𝑚 = 2 or 4. For face- centered-cubic (FCC) materials 𝑚 = 8 is recommended and for body-centered-cubic (BCC) materials 𝑚 = 6 is used. The yield strength of the material is 𝜎y = 𝑘(1 + 𝜀0)𝑛. (22.33.3) Material Models LS-DYNA Theory Manual 22.34 Material Model 34: Fabric The fabric model is a variation on the Layered Orthotropic Composite material model (Material 22) and is valid for only 3 and 4 node membrane elements. This material model is strongly recommended for modeling airbags and seatbelts. In addition to being a constitutive model, this model also invokes a special membrane element formulation that is better suited to the large deformations experienced by fabrics. For thin fabrics, buckling (wrinkling) can occur with the associated inability of the structure to support compressive stresses; a material parameter flag is included for this option. A linear elastic liner is also included which can be used to reduce the tendency for these material/elements to be crushed when the no-compression option is invoked. If the airbag material is to be approximated as an isotropic elastic material, then only one Young’s modulus and Poisson’s ratio should be defined. The elastic approximation is very efficient because the local transformations to the material coordinate system may be skipped. If orthotropic constants are defined, it is very important to consider the orientation of the local material system and use great care in setting up the finite element mesh. If the reference configuration of the airbag is taken as the folded configuration, the geometrical accuracy of the deployed bag will be affected by both the stretching and the compression of elements during the folding process. Such element distortions are very difficult to avoid in a folded bag. By reading in a reference configuration such as the final unstretched configuration of a deployed bag, any distortions in the initial geometry of the folded bag will have no effect on the final geometry of the inflated bag. This is because the stresses depend only on the deformation gradient matrix: 𝐹𝑖𝑗 = 𝜕𝑥𝑖 𝜕𝑋𝑗 , (22.34.1) where the choice of 𝑋𝑗 may coincide with the folded or unfold configurations. It is this unfolded configuration which may be specified here. When the reference geometry is used then the no-compression option should be active. With the reference geometry it is possible to shrink the airbag and then perform the inflation. Although the elements in the shrunken bag are very small, the time step can be based on the reference geometry so a very reasonable time step size is obtained. The reference geometry based time step size is optional in the input. The parameters fabric leakage coefficient, FLC, fabric area coefficient, FAC, and effective leakage area, ELA, for the fabric in contact with the structure are optional for the Wang-Nefske and hybrid inflation models. It is possible for the airbag to be constructed of multiple fabrics having different values of porosity and permeability. LS-DYNA Theory Manual Material Models The gas leakage through the airbag fabric then requires an accurate determination of the areas by part ID available for leakage. The leakage area may change over time due to stretching of the airbag fabric or blockage when the outer surface of the bag is in contact with the structure. LS-DYNA can check the interaction of the bag with the structure and split the areas into regions that are blocked and unblocked depending on whether the regions are in contact or not, respectively. Typically, the parameters, FLC and FAC, must be determined experimentally and their variation with time and pressure are optional inputs that allow for maximum modeling flexibility. Material Models LS-DYNA Theory Manual 22.35 Material Model 35: Kinematic/Isotropic Plastic Green- Naghdi Rate The reader interested in an detailed discussion of the relative merits of various stress rates, especially Jaumann [1911] and Green-Naghdi [1965], is urged to read the work of Johnson and Bammann [1984]. A mathematical description of these two stress rates, and how they are implemented in LS-DYNA, is given in the section entitled Stress Update Overview in this manual. In the cited work by Johnson and Bammann, they conclude that the Green- Naghdi stress rate is to be preferred over all other proposed stress rates, including the most widely used Jaumann rate, because the Green-Naghdi stress rate is based on the notions of However, invariance under superimposed rigid-body motions. implementation of the Green-Naghdi stress rate comes at a significant computational cost compared to the Jaumann stress rate, e.g., see the discussion in this manual in the section entitled Green-Naghdi Stress Rate. Perhaps more importantly, in practical applications there is little if any noted difference in the results generated using either Jaumann or Green-Naghdi stress rate. This is in part due to the fact that the Jaumann stress rate only produces erroneous results2 when linear kinematic hardening is used; the results for isotropic hardening are not affected by the choice of either of these two stress rates. Also in practical applications, the shear strains are rather small, compared to the extensional strains, and if they are not small it is usually the case that the material description, i.e., constitutive model, is not valid for such large shear strains. 2 The results of a simple shear simulation, monotonically increasing shear deformation, produce sinusoidal stress response. LS-DYNA Theory Manual Material Models 22.36 Material Model 36: Barlat’s 3-Parameter Plasticity Model Material model 36 in LS-DYNA aims at modeling sheets with anisotropy under plane stress conditions. It allows the use of the Lankford parameters for the definition of the anisotropic yield surface. The yield condition can be written 𝑓 (𝛔, 𝜀p) = 𝜎eff(𝜎11, 𝜎22, 𝜎12) − 𝜎Y(𝜀p) ≤ 0, (22.36.1) where 𝜎eff(𝜎11, 𝜎22, 𝜎12) = ( 𝐾1 = 𝐾1(𝜎11, 𝜎22, 𝜎12) = |𝐾1 + 𝐾2|𝑚 + 𝜎11 + ℎ𝜎22 |𝐾1 − 𝐾2|𝑚 + 1/𝑚 |2𝐾2|𝑚) (22.36.2) 𝐾2 = 𝐾2(𝜎11, 𝜎22, 𝜎12) = √( 𝜎11 − ℎ𝜎22 ) 2 , + 𝑝2𝜎12 and the hardening of the yield surface is either linear, exponential or determined by a load curve. In the above, the stress components 𝜎11, 𝜎22 and 𝜎12 are with respect to the material coordinate system and 𝜀p denotes the effective plastic strain. The material parameters 𝑎, 𝑐, ℎ and 𝑝 can be determined from the Lankford parameters as described in the LS-DYNA Keyword User’s Manual [Hallquist 2003]. The Lankford parameters, or R-values, are defined as the ratio of instantaneous width change to instantaneous thickness change. That is, assume that the width 𝑊 and thickness 𝑇 are measured as function of strain. Then the corresponding R-value is given by 𝑅 = 𝑑𝑊 𝑑𝜀 𝑑𝑇 𝑑𝜀 /𝑊 /𝑇 . The gradient of the yield surface is denoted ∂𝑓 ∂𝛔 (𝛔) = ∂𝑓 ∂𝜎11 ∂𝑓 ∂𝜎22 ∂𝑓 ∂𝜎12 ⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎛ ⎝ where LS-DYNA Draft (𝛔) (𝛔) (𝛔) ⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎞ ⎠ 𝜕𝑓 𝜕𝜎11 𝜕𝑓 𝜕𝜎22 𝜕𝑓 𝜕𝜎12 (𝜎11, 𝜎22, 𝜎12) (𝜎11, 𝜎22, 𝜎12) (𝜎11, 𝜎22, 𝜎12) , ⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎞ ⎠ = ⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎛ ⎝ Material Models LS-DYNA Theory Manual (𝜎11, 𝜎22, 𝜎12) = 𝜎eff(𝜎11, 𝜎22, 𝜎12)1−𝑚 ⋅ ∂𝜎eff ∂𝜎11 (𝜎11, 𝜎22, 𝜎12) = 𝜕𝑓 𝜕𝜎11 {𝑎(𝐾1 − 𝐾2)|𝐾1 − 𝐾2|𝑚−2 ( 𝑎(𝐾1 + 𝐾2)|𝐾1 + 𝐾2|𝑚−2 ( 𝑐2𝑚𝐾2 𝑚−1 𝜎11 − ℎ𝜎22 } , 4𝐾2 ) + − 𝜎11 − ℎ𝜎22 4𝐾2 𝜎11 − ℎ𝜎22 4𝐾2 + ) + (22.36.4) (𝜎11, 𝜎22, 𝜎12) = 𝜎eff(𝜎11, 𝜎22, 𝜎12)1−𝑚 ℎ ⋅ 𝜕𝜎eff 𝜕𝜎22 (𝜎11, 𝜎22, 𝜎12) = 𝜕𝑓 𝜕𝜎22 {𝑎(𝐾1 − 𝐾2)|𝐾1 − 𝐾2|𝑚−2 ( 𝑎(𝐾1 + 𝐾2)|𝐾1 + 𝐾2|𝑚−2 ( ) + + 𝜎11 − ℎ𝜎22 4𝐾2 𝜎11 − ℎ𝜎22 4𝐾2 − ) − (22.36.5) 𝑐2𝑚𝐾2 𝑚−1 𝜎11 − ℎ𝜎22 } , 4𝐾2 and (𝜎11, 𝜎22, 𝜎12) = 𝜕𝑓 𝜕𝜎12 {−𝑎(𝐾1 − 𝐾2)|𝐾1 − 𝐾2|𝑚−2 + 𝑎(𝐾1 + 𝐾2)|𝐾1 + 𝐾2|𝑚−2 + 𝑐2𝑚𝐾2 𝜎eff(𝜎11, 𝜎22, 𝜎12)1−𝑚 (𝜎11, 𝜎22, 𝜎12) = 𝜕𝜎eff 𝜕𝜎12 𝑝2𝜎12 𝐾2 𝑚−1}. ⋅ (22.36.6) 22.36.1 Material Tangent Stiffness Since the plastic model is associative, the general expression for tangent relating the total strain rate to total stress rate can be found in standard textbooks. Since this situation is rather special we derive it here for the plane stress model presented in the previous section. The elastic stress-strain relation can be written 1 − 𝜈 𝛔̇ = ⎟⎟⎟⎟⎟⎟⎟⎟⎞ 𝜎̇11 𝜎̇22 𝜎̇12 𝜎̇23 𝜎̇13⎠ ⎜⎜⎜⎜⎜⎜⎜⎜⎛ ⎝ = 1 − ν2 ⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎛ ⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎞ 1 − 𝜈 1 − 𝜈 ⎝ = 𝐂ps(𝛆̇ − 𝛆̇p). 2 ⎠ 𝜀̇11 − 𝜀̇11 𝜀̇22 − 𝜀̇22 p ) 2(𝜀̇12 − 𝜀̇12 p ) 2(𝜀̇23 − 𝜀̇23 p )⎠ 2(𝜀̇13 − 𝜀̇13 ⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎞ ⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎛ ⎝ (22.36.7) where 𝐸 is the Young’s modulus, 𝜈 is the Poisson’s ratio and 𝐂ps denotes the plane stress elastic tangential stiffness matrix. The associative flow rule for the plastic strain can be written LS-DYNA Theory Manual Material Models and the consistency condition results in 𝛆̇p = λ̇ ∂𝑓 ∂𝛔 , ∂𝑓 T ∂𝛔 𝛔̇ + ∂𝑓 ∂𝜀p 𝛆̇p = 0. (22.36.8) (22.36.9) For algorithmic consistency, the effective plastic strain rate is defined as 𝜀̇p = 𝜆̇. ∂𝑓 ∂𝛔 and using Equation (22.36.8) and Equation Multiplying Equation (22.36.7) with (22.36.9) gives 𝐂ps𝛆̇ ∂𝑓 ∂𝛔 𝐂ps ∂𝑓 ∂𝛔 . − ∂𝑓 ∂𝜀p λ̇ = ∂𝑓 ∂𝛔 Inserting 𝛆̇p = ∂𝑓 ∂𝛔 into Equation (22.36.7) results in 𝐂ps𝛆̇ ∂𝑓 ∂𝛔 𝐂ps ∂𝑓 ∂𝛔 − ∂𝑓 ∂𝜀p ∂𝑓 ∂𝛔 , 𝐂ps − 𝛔̇ = ⎜⎜⎜⎜⎜⎜⎜⎜⎜⎛ ⎝ } } {𝐂ps ∂𝑓 ∂𝛔 {𝐂ps ∂𝑓 ∂𝛔 𝐂ps ∂𝑓 ∂𝛔 ∂𝑓 ∂𝛔 − ∂𝑓 ∂𝜀p ⎠ ⎟⎟⎟⎟⎟⎟⎟⎟⎟⎞ (22.36.10) (22.36.11) 𝛆̇. (22.36.12) To get the elastic-plastic tangent stiffness tensor in the element coordinate system it needs to be transformed back. Since the elastic tangential stiffness tensor is isotropic with respect to the axis of rotation, the plastic tangent stiffness tensor can be written ps 𝐂plastic = 𝐂ps − ⎜⎜⎜⎜⎜⎜⎜⎜⎜⎛ ⎝ {𝐐𝐂ps ∂𝑓 ∂𝛔 𝐂ps ∂𝑓 ∂𝛔 ∂𝑓 ∂𝛔 } {𝐐𝐂ps ∂𝑓 ∂𝛔 } − ∂𝑓 ∂𝜀p ⎠ ⎟⎟⎟⎟⎟⎟⎟⎟⎟⎞ , (22.36.13) where 𝐐 is the rotation matrix in Voigt form. Material Models LS-DYNA Theory Manual 𝜎22 𝒏(𝑅𝜑) 𝜕𝑓 𝜕𝝈 𝒏(𝑅45) 𝜎𝑌 𝜕𝑓 𝜕𝝈 𝜕𝑓 𝜕𝝈 𝒏(𝑅90) 𝑓 (𝝈, 𝜀𝑝) ≤ 0 𝜎𝑌(𝜀𝑝) 𝛼00, 𝛼45, 𝛼90 changes 𝒏(𝑅00) 𝜕𝑓 𝜕𝝈 𝜎11 90(𝜀𝑝) 𝜎𝑌 45(𝜀𝑝) 𝜎𝑌 00(𝜀𝑝) 𝜎𝑌 𝜀𝑝 22-1 Plastic flow direction (left) and hardening (right) illustrated for variable R-values and hardening. Changes in 𝛼00, 𝛼45 and 𝛼90 come from 22.36.2 Load curves in different directions A project by Fleischer et.al. [2007] resulted in the option HR = 7, see *MAT_036 in LS- DYNA Keyword User’s Manual, which allows for specification of different hardening curves in the three directions corresponding to 0, 45 and 90 degrees. In addition, the R- values in these directions can be specified as functions of plastic strains, both features make up an interesting extension to the standard form of the material model. This section is devoted to the theory of the hardening option while the theory for the R- values follows in the next section. An introductory remark 22.36.2.1 This material typically fits three Lankford parameters and the yield stress in the 00 direction. This fit will result in a non-intuitive effective stress-strain relationship for uniaxial tension in other directions. To explain this we assume that we pull in the 𝜑 direction giving a uniaxial stress value of 𝜎𝜑 and a corresponding plastic strain 𝑝 . The relation between the stress value 𝜎𝜑 and effective stress 𝜎eff is given component 𝜀𝜑 by 𝜎eff = 𝑘𝜑𝜎𝜑 where 𝑘𝜑 = 1 if 𝜑 = 0 but not in general. The plastic work relation, which defines the effective plastic strain for the current material, gives the following expression for the effective plastic strain 𝜀𝑝 = 𝑝 𝜎𝜑 𝜀𝜑 𝜎eff . This means that there is a relationship with a stress-strain hardening curve using the effective stress and strain and a corresponding stress-strain hardening curve using the actual stress and strain values. Assume that a test reveals that the hardening is given by the curve LS-DYNA Theory Manual Material Models 𝜎𝜑 = 𝜎𝜑(𝜀𝜑 𝑝 ) and we want to determine the hardening curve used by LS-DYNA 𝜎eff = 𝜎eff(𝜀𝑝), then using the relationships above yields 𝜎eff(𝜀𝑝) = 𝑘𝜑𝜎𝜑(𝑘𝜑𝜀𝑝). Consequently a user input hardening curve must internally be transformed to an effective hardening curve to be used in the material model to get the desired behavior. Still, the effective plastic strain is not going to be equal to the plastic strain component in the tensile direction and validation of the hardening behavior is not straightforward. Therefore we introduce a new effective plastic strain 𝜀𝑝̃ with evolution given by 𝑑𝜀𝑝̃ 𝑑𝑡 = 𝑘𝜑 𝑑𝜀𝑝 𝑑𝑡 that can be used to verify the hardening relationship. This is actually the von Mises plastic strain in the work hardening sense and is output to the d3plot database as history variable #2 for post-processing. The model 22.36.2.2 The load curve hardening option can be generalized to allow different hardening curves in the 00, 45 and 90 directions, as well as balanced biaxial and shear loading. To this end we let the yield value be given as a convex combination of the hardening curves in each direction as 𝜎𝑌(𝝈, 𝜀𝑝) = 𝛼00𝜎𝑌 00(𝜀𝑝) + 𝛼45𝜎𝑌 45(𝜀𝑝) + 𝛼90𝜎𝑌 90(𝜀𝑝) + 𝛼bi𝜎𝑌 bi(𝜀𝑝) + 𝛼sh𝜎𝑌 sh(𝜀𝑝) 00(𝜀𝑝) is the user defined hardening curve in direction 00, and the others are where 𝜎𝑌 the internal hardening curves in the other directions . The convex parameters must fulfill 0 ≤ 𝛼00 ≤ 1, 0 ≤ 𝛼45 ≤ 1, 0 ≤ 𝛼90 ≤ 1, 0 ≤ 𝛼bi ≤ 1, 0 ≤ 𝛼sh ≤ 1, 𝛼00 + 𝛼45 + 𝛼90 + 𝛼bi + 𝛼sh = 1, and depend on the stress state. Furthermore 𝛼00 = 1 must mean that the stress is uniaxial and is directed in the 00 direction, and that the same thing holds for the other directions. To accomplish this we reason as follows. Let 𝜎̂𝑖𝑗 be the normalized in-plane stress components, i.e., 𝜎̂𝑖𝑗 = 𝜎𝑖𝑗 2 +𝜎22 √𝜎11 2 +2𝜎12 and let 𝜎 be the largest eigenvalue to this matrix and 𝑞𝑖 the associated eigenvector components. Furthermore we define 𝜎𝑣 = (𝜎̂11 + 𝜎̂22)/2 as the normalized volumetric stress and 𝜎𝑑 = √(𝜎̂11−𝜎̂22)2 𝜎𝑑 ≤ 1/√2 and 2 the normalized shear stress, and make a note that 0 ≤ + 𝜎̂12 𝜎𝑑 = 0 → biaxial stress state 𝜎𝑑 = 1/2 → uniaxial stress state 𝜎𝑑 = 1/√2 → shear stress state. 2 is the fraction of stress that is volumetric and 𝑏 = 𝜎 2 an indicator of uniaxial If 𝑎 = 2𝜎𝑣 stress state, then 𝑐 = 𝑎(1 − 4{𝑏 − 1/2}2) is a normalized measure that indicates when Material Models LS-DYNA Theory Manual 2(1 − 𝑞1 the stress is deviatoric/uniaxial or volumetric. That is, 𝑐 = 0 means that the stress is deviatoric or uniaxial and 𝑐 = 1 means that it is volumetric. 2) be the fraction of the eigenvector 𝑞𝑖 that points in the 00 or 90 Now, let 𝑞 = 4𝑞1 direction. That is, 𝑞 = 1 means that the eigenvector points in the 45 direction and 𝑞 = 0 means that it is pointing in either the 00 or 90 direction. Moreover, the same way of reasoning is valid for the eigenvector associated to the smallest eigenvalue. To determine in which direction of 00 or 90 a certain eigenvector is pointing we 2), and deduce that 𝑑 = 1 means that the eigenvector 𝑞𝑖 introduce 𝑑 = 𝑏𝑞1 points in the 00 direction and 𝑑 = 0 means that it is pointing in the 90 direction. We are now ready to give partial expressions for the three uniaxial convex parameters 2 + (1 − 𝑏)(1 − 𝑞1 𝛼̃00 = (1 − 𝑐)𝑑(1 − 𝑞) + 𝑐/4 𝛼̃45 = (1 − 𝑐)𝑞 + 𝑐/2 𝛼̃00 = (1 − 𝑐)(1 − 𝑑)(1 − 𝑞) + 𝑐/4 and these are completed by means of adding the biaxial and shear parts 2) 2 − 1) 𝛼bi = max (0,1 − 4𝜎𝑑 𝛼sh = max (0,4𝜎𝑑 𝛼00 = 𝛼̃00(1 − 𝛼bi − 𝛼sh) 𝛼45 = 𝛼̃45(1 − 𝛼bi − 𝛼sh) 𝛼90 = 𝛼̃90(1 − 𝛼bi − 𝛼sh) This set of parameters fulfills the requirements mentioned above and allows for a decent expression for a directional dependent yield stress. In the consistency condition we do not consider the derivatives of the convex parameters with respect to the stress, as we assume that these will not have a major impact on convergence. 22.36.3 Variable Lankford parameters The R-values are supposed to be variable with deformation, and we let 𝑅00(𝜀𝑝), 𝑅45(𝜀𝑝) and 𝑅90(𝜀𝑝) be the internal load curves that are transformed from the ones given by the user. Then we define the directional dependent R-value according to 𝑅(𝝈, 𝜀𝑝) = 𝛼00𝑅00(𝜀𝑝) + 𝛼45𝑅45(𝜀𝑝) + 𝛼90𝑅90(𝜀𝑝) using the same set of convex parameters as in the previous section. A generalized relation for the R-value in terms of the stress can be given as (𝜎̂22 + {𝜎̂11 + 𝜎̂22}𝑅)𝑛1 + (𝜎̂11 + {𝜎̂11 + 𝜎̂22}𝑅)𝑛2 − 𝜎̂12𝑛4 = 0, where 𝜎̂𝑖𝑗 are the normalized stress components, 𝑛𝑖 is the direction of plastic flow and where we have suppressed the dependence of stress and plastic strain in 𝑅. By setting ∆𝑛1 = 𝑛1 − 𝜕𝑓 𝜕𝜎11 , ∆𝑛2 = 𝑛2 − 𝜕𝑓 𝜕𝜎22 , ∆𝑛4 = 𝑛4 − 𝜕𝑓 𝜕𝜎12 and ∆𝑅 = 𝑅(𝜀𝑝) − 𝑅(0) we can simplify this equation as (𝜎̂22 + {𝜎̂11 + 𝜎̂22}𝑅)∆𝑛1 + (𝜎̂11 + {𝜎̂11 + 𝜎̂22}𝑅)∆𝑛2 − 𝜎̂12∆𝑛4 = −( 𝜕𝑓 𝜕𝜎11 + 𝜕𝑓 𝜕𝜎22 ){𝜎̂11 + 𝜎̂22}∆𝑅 LS-DYNA Theory Manual Material Models assuming that the relation already holds for the yield surface normal and R-value in the reference configuration. This equation is complemented with a consistency condition of the plastic flow 𝜎̂11∆𝑛1 + 𝜎̂22∆𝑛2 + 𝜎̂12∆𝑛4 = 0. These two equations are linearly independent if and only if {𝜎̂11 + 𝜎̂22}√(𝜎̂11−𝜎̂22)2 + 𝜎̂12 2 ≠ 0 and then the equation −𝜎̂12∆𝑛1 + 𝜎̂12∆𝑛2 + (𝜎̂11 − 𝜎̂22)∆𝑛4 = 0 can be used to complement the previous two. This defines a system of equations that can be used to solve in least square sense for the perturbation ∆𝑛𝑖 of the yield surface normal to get the R-value of interest. To avoid numerical problems and make the perturbation continuous with respect to the stress, the right hand side of the first equation is changed to 𝜕𝑓 𝜕𝜎11 ){𝜎̂11 + 𝜎̂22}((𝜎̂11 − 𝜎̂22)2 + 4𝜎̂12 2 )∆𝑅. 𝜕𝑓 𝜕𝜎22 −( + This results in a non-associated flow rule, meaning that the plastic flow is not in the direction of the yield surface normal. Again, we don’t take any special measures into account for the stress return algorithm as we believe that the perturbation of the normal is small enough not to deteriorate convergence. In figure 22-1 the plastic flow direction is illustrated as function of the stress on the yield surface. Material Models LS-DYNA Theory Manual 22.37 Material Model 37: Transversely Anisotropic Elastic- Plastic This fully iterative plasticity model is available only for shell elements. The input parameters for this model are: Young’s modulus 𝐸; Poisson’s ratio 𝜐; the yield stress; the tangent modulus 𝐸t; and the anisotropic hardening parameter 𝑅. Consider Cartesian reference axes which are parallel to the three symmetry planes of anisotropic behavior. Then the yield function suggested by Hill [1948] can be written F(𝜎22 − 𝜎33)2 + G(𝜎33 − 𝜎11)2 + H(𝜎11 − 𝜎22)2 + 2L𝜎23 where 𝜎y1, 𝜎y2, and 𝜎y3, are the tensile yield stresses and 𝜎y12, 𝜎y23, and 𝜎y31 are the shear yield stresses. The constants F, G, H, L, M, and N are related to the yield stress by 2 − 1 = 0,(22.37.1) 2 + 2M𝜎31 2 + 2N𝜎12 2L = 2M = 2N = 2F = 2G = 2H = 𝜎y23 2 𝜎y31 2 𝜎y12 2 + 𝜎y2 2 + 𝜎y3 2 + 𝜎y1 2 − 𝜎y3 2 − 𝜎y1 2 − 𝜎y2 2 𝜎y1 2 𝜎y2 2 . 𝜎y3 The isotropic case of von Mises plasticity can be recovered by setting and F = G = H = L = M = N = 2, 2𝜎y 2. 2𝜎y (22.37.2) (22.37.3) (22.37.4) For the particular case of transverse anisotropy, where properties do not vary in the 𝑥1 − 𝑥2 plane, the following relations hold: LS-DYNA Theory Manual Material Models F = 2G = 2H = N = 2 − 𝜎y 2 − 𝜎y 𝜎y3 2 𝜎y3 2 , 𝜎y3 where it has been assumed that 𝜎y1 = 𝜎y2 = 𝜎y. Letting K = 𝜎y 𝜎y3 , the yield criterion can be written 𝑭(𝛔) = 𝜎e = 𝜎y, where 𝐹(𝛔) ≡ [𝜎11 2 + 𝜎22 2 + K2𝜎33 2 − K2𝜎33(𝜎11 + 𝜎22) − (2 − K2)𝜎11𝜎22 +2L𝜎y 2(𝜎23 2 + 𝜎31 2 ) + 2 (2 − 2 ] K2) 𝜎12 2⁄ . (22.37.5) (22.37.6) (22.37.7) The rate of plastic strain is assumed to be normal to the yield surface so 𝜀̇𝑖𝑗 p is found from p = λ 𝜀̇𝑖𝑗 ∂𝐹 ∂𝜎𝑖𝑗 . (22.37.8) Now consider the case of plane stress, where 𝜎33 = 0. Also, define the anisotropy input parameter 𝑅 as the ratio of the in-plane plastic strain rate to the out-of-plane plastic strain rate: It then follows that 𝑅 = 𝜀̇22 p . 𝜀̇33 𝑅 = K2 − 1. (22.37.9) (22.37.10) Using the plane stress assumption and the definition of 𝑅, the yield function may now be written F(𝛔) = [𝜎11 2 + 𝜎22 2 − 2R R + 1 𝜎11𝜎22 + 2 2R + 1 R + 1 2⁄ . 2 ] 𝜎12 (22.37.11) Material Models LS-DYNA Theory Manual 22.38 Material Model 38: Blatz-Ko Compressible Foam 𝑊(𝐼1, 𝐼2, 𝐼3) = 𝐼2 𝐼3 where 𝜇 is the shear modulus and 𝐼1, 𝐼2, and 𝐼3 are the strain invariants. Blatz and Ko [1962] suggested this form for a 47 percent volume polyurethane foam rubber with a Poisson’s ratio of 0.25. The second Piola-Kirchhoff stresses are given as + 2√𝐼3 − 5), (22.38.1) ( 𝑆𝑖𝑗 = 𝜇 [(𝐼𝛿𝑖𝑗 − 𝐺𝑖𝑗) 𝐼3 + (√𝐼3 − ) 𝐺𝑖𝑗], 𝐼2 𝐼3 (22.38.2) where 𝐺𝑖𝑗 = stress tensor: 𝜕𝑥𝑘 𝜕𝑋𝑖 𝜕𝑥𝑘 𝜕𝑋𝑗 , 𝐺𝑖𝑗 = 𝜕𝑋𝑖 𝜕𝑥𝑘 𝜕𝑋𝑗 𝜕𝑥𝑘 , after determining 𝑆𝑖𝑗, it is transformed into the Cauchy σ𝑖𝑗 = 𝜌0 𝜕𝑥𝑖 𝜕𝑋𝑘 𝜕𝑥𝑗 𝜕𝑋𝑙 𝑆𝑘𝑙, (22.38.3) where 𝜌0 and 𝜌 are the initial and current density, respectively. LS-DYNA Theory Manual Material Models 22.39 Material Model 39: Transversely Anisotropic Elastic- Plastic With FLD See Material Model 37 for the similar model theoretical basis. The first history variable is the maximum strain ratio defined by: 𝜀majorworkpiece εmajorfld (22.39.1) corresponding to 𝜀minorworkpiece. This history variable replaces the effective plastic strain in the output. Plastic strains can still be obtained but one additional history variable must be written into the D3PLOT database. The strains on which these calculations are based are integrated in time from the strain rates: mjr = 0 mjr Plane Strain mnr mjr mnr mjr Draw Stretch 80 70 60 50 40 30 20 10 % -50 -40 -30 -20 -10 10 20 30 40 50 % Minor Strain Figure 22.39.1. Flow limit diagram. 𝑛+1 = 𝜀𝑖𝑗 𝜀𝑖𝑗 𝑛 + 𝜀𝑖𝑗 ∇𝑛+1 2⁄ Δ𝑡𝑛+1 2⁄ , (22.39.2) and are stored as history variables. The resulting strain measure is logarithmic. Material Models LS-DYNA Theory Manual 22.40 Material Model 42: Planar Anisotropic Plasticity Model This model is built into LS-DYNA as a user material model for modeling plane stress anisotropic plasticity in shells. Please note that only three cards are input here. The orthotropic angles must be defined later as for all materials of this type. This model is currently not vectorized. This is an implementation of an anisotropic plasticity model for plane stress where the flow rule, see Material Type 37, simplifies to: 𝐹(𝜎22)2 + 𝐺(𝜎11)2 + 𝐻(𝜎11 − 𝜎22)2 + 2𝑁𝜎12 2 − 1 = 0. (22.40.1) The anisotropic parameters R00, R45, and R90 are defined in terms of 𝐹, 𝐺, 𝐻, and 𝑁 as [Hill, 1989]: 2𝑅00 = 2𝑅45 = 2𝑅90 = , 2𝑁 (𝐹 + 𝐺) . − 1, (22.40.2) The yield function for this model is given as: 𝜎y = 𝐴𝜀𝑚𝜀̇𝑛. (22.40.3) To avoid numerical problems the minimum strain rate, 𝜀̇min must be defined and the initial yield stress 𝜎0 is calculated as 𝜎0 = 𝐴𝜀0 𝑚𝜀̇min 𝑛 = 𝐸𝜀0, 𝜀0 = ( 𝑚−1 . 𝑛 ) 𝐴𝜀̇min (22.40.4) (22.40.5) LS-DYNA Theory Manual Material Models 22.41 Material Model 51: Temperature and Rate Dependent Plasticity The kinematics associated with the model are discussed in references [Hill 1948, Bammann and Aifantis 1987, Bammann 1989]. The description below is taken nearly verbatim from Bammann [Hill 1948]. With the assumption of linear elasticity we can write, = 𝜆tr(𝐃e)𝟏 + 2𝜇𝐃e, where, the Cauchy stress 𝛔 is convected with the elastic spin 𝐖e as, = 𝛔̇ − 𝐖e𝛔 + 𝛔𝐖e. (22.41.1) (22.41.2) This is equivalent to writing the constitutive model with respect to a set of directors whose direction is defined by the plastic deformation [Bammann and Aifantis 1987, Bammann and Johnson 1987]. Decomposing both the skew symmetric and symmetric parts of the velocity gradient into elastic and plastic parts we write for the elastic stretching 𝐃e and the elastic spin 𝐖e, 𝐃e = 𝐃 − 𝐃p − 𝐃th, 𝐖e = 𝐖 = 𝐖p. (22.41.3) Within this structure it is now necessary to prescribe an equation for the plastic spin 𝐖p in addition to the normally prescribed flow rule for 𝐃p and the stretching due to the thermal expansion 𝐃th. As proposed, we assume a flow rule of the form, 𝐃p = 𝑓 (𝑇) sinh [ |𝛏| − 𝜅 − 𝑌(𝑇) 𝑉(𝑇) ] 𝛏′ ∣𝛏′∣ , (22.41.4) where 𝑇 is the temperate, 𝜅 is the scalar hardening variable, 𝛏′ is the difference between the deviatoric Cauchy stress 𝛔′ and the tensor variable 𝛂′, 𝛏′ = 𝛔′ − 𝛂′, (22.41.5) and 𝑓 (𝑇), 𝑌(𝑇), 𝑉(𝑇) are scalar functions whose specific dependence upon the temperature is given below. Assuming isotropic thermal expansion, and introducing the expansion coefficient 𝐴̇, the thermal stretching can be written, 𝐃th = 𝐴̇𝑇̇𝟏. (22.41.6) The evolution of the internal variables 𝛼 and 𝜅 are prescribed in a hardening minus recovery format as, = ℎ(𝑇)𝐃p − [𝑟d (T) ∣𝐃p∣ + 𝑟s(𝑇)] |𝛂|𝛂, (22.41.7) Material Models LS-DYNA Theory Manual 𝜅̇ = 𝐻(𝑇)𝐃p − [𝑅d(𝑇) ∣𝐃p∣ − 𝑅s(𝑇)]𝜅2, (22.41.8) where ℎ and 𝐻 are the hardening moduli, 𝑟𝑠(𝑇) and 𝑅s(𝑇) are scalar functions describing the diffusion controlled ‘static’ or ‘thermal’ recovery, and 𝑟d(𝑇) and 𝑅d(𝑇) are the functions describing dynamic recovery. If we assume that 𝐖p = 0, we recover the Jaumann stress rate which results in the prediction of an oscillatory shear stress response in simple shear when coupled with a Prager kinematic hardening assumption [Johnson and Bammann 1984]. Alternatively we can choose, 𝐖p = 𝐑T𝐔̇ 𝐔−1𝐑, (22.41.9) which recovers the Green-Naghdi rate of Cauchy stress and has been shown to be equivalent to Mandel’s isoclinic state [Bammann and Aifantis 1987]. The model employing this rate allows a reasonable prediction of directional softening for some materials but in general under-predicts the softening and does not accurately predict the axial stresses which occur in the torsion of the thin walled tube. The final equation necessary to complete our description of high strain rate deformation is one which allows us to compute the temperature change during the deformation. In the absence of a coupled thermomechanical finite element code we assume adiabatic temperature change and follow the empirical assumption that 90 - 95% of the plastic work is dissipated as heat. Hence, 𝑇̇ = 0.9 𝜌𝐶v (𝛔 ⋅ 𝐃p), (22.41.10) where 𝜌 is the density of the material and 𝐶v the specific heat. In terms of the input parameters the functions defined above become: 𝑉(𝑇) = C1 ∙ exp(−C2/𝑇) 𝑌(𝑇) = C3 ∙ exp(C4/𝑇) 𝑓 (𝑇) = C5 ∙ exp(−C6/𝑇) 𝑟𝑑(𝑇) = C7 ∙ exp(−C8/𝑇) and the heat generation coefficient is ℎ(𝑇) = C9 ∙ exp(C10/𝑇) 𝑟𝑠(𝑇) = C11 ∙ exp(−C12/𝑇) 𝑅𝑑(𝑇) = C13 ∙ exp(−C14/𝑇) 𝐻(𝑇) = C15 ∙ exp(C16/𝑇) 𝑅𝑠(𝑇) = C17 ∙ exp(−C18/𝑇) 𝐻𝐶 = 0.9 𝜌𝐶𝑉 . (22.41.11) LS-DYNA Theory Manual Material Models 22.42 Material Model 52: Sandia’s Damage Model The evolution of the damage parameter, 𝜙, is defined by [Bammann, et. al., 1990] 𝜙̇ = 𝛽 [ (1 − 𝜙)𝑁 − (1 − 𝜙)] ∣Dp∣ , in which where 𝑝 is the pressure and 𝜎̅̅̅̅̅ is the effective stress. 𝛽 = sin [ 2(2𝑁 − 1)𝑝 (2𝑁 − 1)𝜎̅̅̅̅̅ ], (22.42.1) (22.42.2) Material Models LS-DYNA Theory Manual 22.43 Material Model 53: Low Density Closed Cell Polyurethane Foam A rigid, low density, closed cell, polyurethane foam model developed at Sandia Laboratories [Neilsen et al., 1987] has been recently implemented for modeling impact limiters in automotive applications. A number of such foams were tested at Sandia and reasonable fits to the experimental data were obtained. In some respects this model is similar to the crushable honeycomb model type 26 in that the components of the stress tensor are uncoupled until full volumetric compaction is achieved. However, unlike the honeycomb model this material possesses no directionality but includes the effects of confined air pressure in its overall response characteristics. where 𝜎𝑖𝑗 sk is the skeletal stress and 𝜎 air is the air pressure computed from the equation: 𝜎𝑖𝑗 = 𝜎𝑖𝑗 sk − δ𝑖𝑗𝜎 air, (22.43.1) 𝜎 air = − 𝑝0𝛾 1 + 𝛾 − 𝜙 , (22.43.2) where 𝑝0 is the initial foam pressure usually taken as the atmospheric pressure and 𝛾 defines the volumetric strain 𝛾 = 𝑉 − 1 + 𝛾0, (22.43.3) where 𝑉 is the relative volume and 𝛾0 is the initial volumetric strain which is typically zero. The yield condition is applied to the principal skeletal stresses which are updated independently of the air pressure. We first obtain the skeletal stresses: 𝜎𝑖𝑗 sk = 𝜎𝑖𝑗 + 𝜎𝑖𝑗𝜎 air, and compute the trial stress, 𝛔𝑖 skt skt = 𝜎𝑖𝑗 𝜎𝑖𝑗 sk + 𝐸𝜀̇𝑖𝑗Δ𝑡, (22.43.4) (22.43.5) where 𝐸 is Young’s modulus. Since Poisson’s ratio is zero, the update of each stress component is uncoupled and 2𝐺 = 𝐸 where 𝐺 is the shear modulus. The yield condition is applied to the principal skeletal stresses such that if the magnitude of a principal trial stress component, 𝛔𝑖 skt, exceeds the yield stress, 𝜎y, then sk = min(𝜎y, ∣𝛔𝑖 𝛔𝑖 skt∣) skt . skt∣ 𝛔𝑖 ∣𝛔𝑖 The yield stress is defined by 𝜎y = 𝑎 + 𝑏(1 + 𝑐𝛾), 22-134 (Material Models) (22.43.6) LS-DYNA Theory Manual Material Models where 𝑎, 𝑏, and 𝑐 are user defined input constants. After scaling the principal stresses they are transformed back into the global system and the final stress state is computed sk − 𝛿𝑖𝑗𝜎 air. 𝜎𝑖𝑗 = 𝜎𝑖𝑗 (22.43.8) Material Models LS-DYNA Theory Manual 22.44 Material Models 54 and 55: Enhanced Composite Damage Model These models are very close in their formulations. Material 54 uses the Chang matrix failure criterion (as Material 22), and material 55 uses the Tsay-Wu criterion for matrix failure. Arbitrary orthothropic materials, e.g., unidirectional layers in composite shell structures can be defined. Optionally, various types of failure can be specified following either the suggestions of [Chang and Chang, 1984] or [Tsai and Wu, 1981]. In addition special measures are taken for failure under compression. See [Matzenmiller and Schweizerhof, 1990]. This model is only valid for thin shell elements. The Chang/Chang criteria is given as follows: for the tensile fiber mode, 𝜎aa > 0 then 𝑒f 2 = ( 𝜎aa Xt ) + 𝛽 ( ) 𝜎𝑎𝑏 𝑆𝑐 − 1 {≥ 0 failed , < 0 elastic for the compressive fiber mode, Ea = Eb = Gab = νba = νab = 0, 𝜎aa < 0 then 𝑒c 2 = ( 𝜎aa Xc ) − 1 {≥ 0 failed < 0 elastic , for the tensile matrix mode, Ea = νba = νab = 0, 𝜎bb > 0 then 𝑒m 2 = ( 𝜎bb Yt ) + ( 𝜎ab Sc ) − 1 {≥ 0 failed , < 0 elastic and for the compressive matrix mode, Eb = νba = 0 → Gab = 0, (22.44.1) (22.44.2) (22.44.3) (22.44.4) (22.44.5) (22.44.6) 𝜎bb < 0 then 𝑒d 2 = ( 𝜎bb 2Sc ) + ) Yc 2Sc ⎢⎡( ⎣ − 1 ⎥⎤ 𝜎bb Yc ⎦ + ( ) 𝜎ab Sc − 1 {≥ 0 failed < 0 elastic , (22.44.7) Eb = νba = νab = 0 ⇒ Gab = 0 XC = 2Yc, for 50% fiber volume . (22.44.8) In the Tsay/Wu criteria the tensile and compressive fiber modes are treated as in the Chang/Chang criteria. The failure criterion for the tensile and compressive matrix mode is given as: LS-DYNA Theory Manual Material Models 2 = 𝑒md 𝜎bb YcYt + ( 𝜎ab Sc ) + (Yc − Yt) 𝜎bb YcYt − 1 {≥ 0 failed < 0 elastic . (22.44.9) For 𝛽 = 1 we get the original criterion of Hashin [1980] in the tensile fiber mode. For 𝛽 = 0, we get the maximum stress criterion which is found to compare better to experiments. Failure can occur in any of four different ways: 1. 2. 3. 4. If DFAILT is zero, failure occurs if the Chang/Chang failure criterion is satisfied in the tensile fiber mode. If DFAILT is greater than zero, failure occurs if the tensile fiber strain is greater than DFAILT or less than DFAILC. If EFS is greater than zero, failure occurs if the effective strain is greater than EFS. If TFAIL is greater than zero, failure occurs according to the element time step as described in the definition of TFAIL above. When failure has occurred in all the composite layers (through-thickness integration points), the element is deleted. Elements which share nodes with the deleted element become “crashfront” elements and can have their strengths reduced by using the SOFT parameter with TFAIL greater than zero. Information about the status in each layer (integration point) and element can be plotted using additional integration point variables. The number of additional integration point variables for shells written to the LS-DYNA database is input by the *DATABASE_BINARY definition as variable NEIPS. For Models 54 and 55 these additional variables are tabulated below (i = shell integration point): History Variable Description Value 1. 𝑒𝑓 (𝑖) 2. 𝑒𝑐(𝑖) 3. 𝑒𝑚(𝑖) 4. 𝑒𝑑(𝑖) tensile fiber mode compressive fiber mode tensile matrix mode compressive mode matrix 5. 𝑒𝑓𝑎𝑖l max[𝑒𝑓 (𝑖𝑝)] 6. 𝑑𝑎𝑚 damage parameter 1 – elastic 0 – failed -1 - element intact 10-8 - element in crashfront +1 - element failed LS-PREPOST History Variable 1 2 3 4 5 Material Models LS-DYNA Theory Manual The following components, defined by the sum of failure indicators over all through-thickness integration points, are stored as element component 7 instead of the effective plastic strain.: 𝑛𝑖𝑝 Description 𝑛𝑖𝑝 ∑ 𝑒𝑓 (𝑖) 𝑖=1 𝑛𝑖𝑝 ∑ 𝑒𝑐(𝑖) 𝑖=1 𝑛𝑖𝑝 ∑ 𝑐𝑚(𝑖) 𝑖=1 𝑛𝑖𝑝 𝑛𝑖𝑝 Integration point 1 2 LS-DYNA Theory Manual Material Models 22.45 Material Model 57: Low Density Urethane Foam The urethane foam model is available to model highly compressible foams such as those used in seat cushions and as padding on the Side Impact Dummy (SID). The compressive behavior is illustrated in Figure 22.45.1 where hysteresis on unloading is shown. This behavior under uniaxial loading is assumed not to significantly couple in the transverse directions. In tension the material behaves in a linear fashion until tearing occurs. Although our implementation may be somewhat unusual, it was first motivated by Shkolnikov [1991] and a paper by Storakers [1986]. The recent additions necessary to model hysteretic unloading and rate effects are due to Chang, et al., [1994]. These latter additions have greatly expanded the usefulness of this model. The model uses tabulated input data for the loading curve where the nominal stresses are defined as a function of the elongations, 𝜀𝑖, which are defined in terms of the principal stretches, 𝜆𝑖, as: 𝜀𝑖 = 𝜆 𝑖 − 1. (22.45.1) The stretch ratios are found by solving for the eigenvalues of the left stretch tensor, 𝑉𝑖𝑗, which is obtained via a polar decomposition of the deformation gradient matrix, 𝐹𝑖𝑗: 𝐹𝑖𝑗 = 𝑅𝑖𝑘𝑈𝑘𝑗 = 𝑉𝑖𝑘𝑅𝑘𝑗. (22.45.2) The update of 𝑉𝑖𝑗 follows the numerically stable approach of Taylor and Flanagan [1989]. After solving for the principal stretches, the elongations are computed and, if the elongations are compressive, the corresponding values of the nominal stresses, 𝜏𝑖 are interpolated. If the elongations are tensile, the nominal stresses are given by Typical unloading curves determined by the hysteretic unloading factor. With the shape factor equal to unity. Typical unloading for a large shape factor, e.g. 5.0-8.0, and a small hystereticfactor, e.g., 0.010. Unloading curves Strain Strain Figure 22.45.1. Behavior of the low-density urethane foam model. Material Models LS-DYNA Theory Manual 𝜏𝑖 = 𝐸𝜀𝑖. The Cauchy stresses in the principal system become 𝜎𝑖 = 𝜏𝑖 𝜆𝑗𝜆𝑘 . (22.45.3) (22.45.4) The stresses are then transformed back into the global system for the nodal force calculations. When hysteretic unloading is used, the reloading will follow the unloading curve if the decay constant, 𝛽, is set to zero. If 𝛽 is nonzero the decay to the original loading curve is governed by the expression: 1 − 𝑒−𝛽𝑡. (22.45.5) The bulk viscosity, which generates a rate dependent pressure, may cause an unexpected volumetric response and, consequently, it is optional with this model. Rate effects are accounted for through linear viscoelasticity by a convolution integral of the form r = ∫ 𝑔𝑖𝑗𝑘𝑙 𝜎𝑖𝑗 where 𝑔𝑖𝑗𝑘𝑙(𝑡 − 𝜏) is the relaxation function. The stress tensor, 𝜎𝑖𝑗 determined from the foam, 𝜎𝑖𝑗 summation of the two contributions: (𝑡 − 𝜏) r , augments the stresses f ; consequently, the final stress, 𝜎𝑖𝑗, is taken as the (22.45.6) 𝑑𝜏, ∂𝜀𝑘𝑙 ∂𝜏 𝜎𝑖𝑗 = 𝜎𝑖𝑗 r . f + 𝜎𝑖𝑗 (22.45.7) Since we wish to include only simple rate effects, the relaxation function is represented by one term from the Prony series: given by, 𝑔(𝑡) = 𝛼0 + ∑ α𝑚 𝑚=1 𝑒−𝛽𝑡, 𝑔(𝑡) = 𝐸d𝑒−𝛽1𝑡. (22.45.8) (22.45.9) This model is effectively a Maxwell fluid which consists of a damper and spring in series. We characterize this in the input by a Young's modulus, 𝐸d, and decay constant, 𝛽1. The formulation is performed in the local system of principal stretches where only the principal values of stress are computed and triaxial coupling is avoided. Consequently, the one-dimensional nature of this foam material is unaffected by this addition of rate effects. The addition of rate effects necessitates twelve additional LS-DYNA Theory Manual Material Models history variables per integration point. The cost and memory overhead of this model comes primarily from the need to “remember” the local system of principal stretches. Viscous damping is implemented by incrementation of the principal stress components. Firstly, we let 𝑎 = 𝑐𝜌𝜇𝐿𝑒 1 + 𝛾 , (22.45.10) where 𝑐, 𝜌, 𝜇, 𝐿𝑒 and 𝛾 respectively denote the material sound speed, density, viscous The coefficient, element characteristic incremental stress components due to viscous damping are then given by length and element volumetric strain. Δ𝜎𝑖 = 𝑎 ( 𝜀̇𝑖 − 𝜀̇𝑚 1 + 𝜈 + 𝜀̇𝑚 1 − 2𝜈 ) 𝑖 = 1,2,3 and Δ𝜎𝑖 = 𝑎𝜀̇𝑖 2(1 + 𝜈) 𝑖 = 4,5,6, where 𝜀̇𝑖 are the strain rates and 𝜀̇𝑚 = ∑ 𝜀̇𝑖 𝑖=1 3⁄ . (22.45.11) (22.45.12) Material Models LS-DYNA Theory Manual 22.46 Material Model 58: Laminated Composite Fabric Parameters to control failure of an element layer are: ERODS, the maximum effective strain, i.e., maximum 1 = 100% straining. The layer in the element is completely removed after the maximum effective strain (compression/tension including shear) is reached. The stress limits are factors used to limit the stress in the softening part to a given value, 𝜎min = SLIMxx ⋅ strength, (22.46.1) thus, the damage value is slightly modified such that elastoplastic like behavior is achieved with the threshold stress. As a factor for SLIMxx a number between 0.0 and 1.0 is possible. With a factor of 1.0, the stress remains at a maximum value identical to the strength, which is similar to ideal elastoplastic behavior. For tensile failure a small value for SLIMTx is often reasonable; however, for compression SLIMCx = 1.0 is preferred. This is also valid for the corresponding shear value. If SLIMxx is smaller than 1.0 then localization can be observed depending on the total behavior of the lay- up. If the user is intentionally using SLIMxx < 1.0, it is generally recommended to avoid a drop to zero and set the value to something in between 0.05 and 0.10. Then elastoplastic behavior is achieved in the limit which often leads to less numerical problems. Defaults for SLIMXX = 1.0E-8. The crashfront-algorithm is started if and only if a value for TSIZE (time step size, with element elimination after the actual time step becomes smaller than TSIZE) is input . The damage parameters can be written to the postprocessing database for each integration point as the first three additional element variables and can be visualized. Material models with FS = 1 or FS = −1 are favorable for complete laminates and fabrics, as all directions are treated in a similar fashion. For material model FS = 1 an interaction between normal stresses and shear stresses is assumed for the evolution of damage in the a- and b- directions. For the shear damage is always the maximum value of the damage from the criterion in a- or b- direction is taken. For material model FS = −1 it is assumed that the damage evolution is independent of any of the other stresses. A coupling is present only via the elastic material parameters and the complete structure. LS-DYNA Theory Manual Material Models SC TAU1 SLIMS*SC GAMMA1 GMS Figure 22.46.1. Stress-strain diagram for shear. In tensile and compression directions and in a- as well as in b- direction, different failure surfaces can be assumed. The damage values, however, increase only when the loading direction changes. Special control of shear behavior of fabrics For fabric materials a nonlinear stress strain curve for the shear part of failure surface FS = −1 can be assumed as given below. This is not possible for other values of FS. The curve, shown in Figure 22.46.1, is defined by three points: • the origin (0,0) is assumed, • the limit of the first slightly nonlinear part (must be input), stress (TAU1) and strain (GAMMA1), see below. • the shear strength at failure and shear strain at failure. In addition a stress limiter can be used to keep the stress constant via the SLIMS parameter. This value must be less than or equal to 1.0 and positive, which leads to an elastoplastic behavior for the shear part. The default is 1.0E-08, assuming almost brittle failure once the strength limit SC is reached. Material Models LS-DYNA Theory Manual 22.47 Material Model 60: Elastic With Viscosity This material model was developed to simulate the forming of glass products (e.g., car windshields) at high temperatures. Deformation is by viscous flow but elastic deformations can also be large. The material model, in which the viscosity may vary with temperature, is suitable for treating a wide range of viscous flow problems and is implemented for brick and shell elements. Volumetric behavior is treated as linear elastic. The deviatoric strain rate is considered to be the sum of elastic and viscous strain rates: 𝛆̇′total = 𝛆̇′elastic + 𝛆̇′ viscous = 𝛔̇′ 2𝐺 + 𝛔̇′ 2𝜈 , (22.47.1) where 𝐺 is the elastic shear modulus, 𝜈 is the viscosity coefficient. The stress increment over one time step 𝑑𝑡 is 𝑑𝛔′ = 2𝐺𝛆̇′total𝑑𝑡 − 𝑑𝑡𝛔′. (22.47.2) The stress before the update is used for 𝛔′. For shell elements, the through- thickness strain rate is calculated as follows 𝑑𝜎33 = 0 = 𝐾(𝜀̇11 + 𝜀̇22 + 𝜀̇33)𝑑𝑡 + 2𝐺𝜀̇′33 𝑑𝑡 − 𝑑𝑡σ′ 33, (22.47.3) where the subscript 𝑖𝑗 = 33 denotes the through-thickness direction and 𝐾 is the elastic bulk modulus. This leads to: 𝜀̇33 = −a(𝜀̇11 + 𝜀̇22) + 𝑏𝑝, 𝑎 = 𝐾 − 2 𝐾 + 4 , 𝑏 = 𝐺𝑑𝑡 𝜐(𝐾 + 4 , 𝐺) (22.47.4) (22.47.5) (22.47.6) in which 𝑝 is the pressure defined as the negative of the hydrostatic stress. LS-DYNA Theory Manual Material Models 22.48 Material Model 61: Maxwell/Kelvin Viscoelastic with Maximum Strain The shear relaxation behavior is described for the Maxwell model by: 𝐺(𝑡) = G∞ + (G0 − G∞)𝑒−𝛽𝑡. A Jaumann rate formulation is used ∇ 𝑠′𝑖𝑗 = 2 ∫ 𝐺(𝑡 − 𝜏)𝜀′̇ 𝑖𝑗(𝜏)𝑑𝑡 , (22.48.1) (22.48.2) ∇ where the prime denotes the deviatoric part of the stress rate, 𝑠′𝑖𝑗 deviatoric strain rate. , and 𝜀̇′𝑖𝑗 is the For the Kelvin model the stress evolution equation is defined as: 𝑠 ̇𝑖𝑗 + 𝑠𝑖𝑗 = (1 + 𝛿𝑖𝑗)G0𝜀′̇ 𝑖𝑗 + (1 + 𝛿𝑖𝑗) G∞ 𝜀′𝑖𝑗, (22.48.3) where 𝛿𝑖𝑗 is the Kronecker delta, G0 is the instantaneous shear modulus, G∞is the long term shear modulus, and τ is the decay constant. The pressure is determined from the bulk modulus and the volumetric strain: where 𝑝 = −𝐾𝜀v, 𝜀v = ln ( 𝑉0 ), (22.48.4) (22.48.5) defines the logarithmic volumetric strain from the relative volume. Bandak’s [1991] calculation of the total strain tensor, 𝜀𝑖𝑗, for output uses an incremental update based on Jaumann rate: 𝑛+1 = 𝜀𝑖𝑗 𝜀𝑖𝑗 𝑛 + 𝑟𝑖𝑗 𝑛 + 𝜀𝑖𝑗 𝛻𝑛+1 2⁄ 𝛥𝑡𝑛+1 2⁄ , where 𝑛+1 2⁄ 𝛥𝜀𝑖𝑗 𝑛+1 2⁄ 𝛥𝑡𝑛+1 2⁄ , = 𝜀̇𝑖𝑗 and 𝑟𝑖𝑗 𝑛 gives the rotation of the stain tensor at time 𝑡𝑛 to the configuration at 𝑡𝑛+1 𝑛 = (𝜀𝑖𝑝 𝑟𝑖𝑗 𝑛 𝜔𝑝𝑗 𝑛+1 2⁄ + 𝜀𝑗𝑝 𝑛 𝜔𝑝𝑖 𝑛+1 2⁄ ) 𝛥𝑡𝑛+1 2⁄ . (22.48.6) (22.48.7) (22.48.8) Material Models LS-DYNA Theory Manual 22.49 Material Model 62: Viscous Foam This model was written to represent the energy absorbing foam found on certain crash dummies, i.e., the ‘Confor Foam’ covering the ribs of the Eurosid dummy. The model consists of a nonlinear elastic stiffness in parallel with a viscous damper. A schematic is shown in Figure 22.49.1. The elastic stiffness is intended to limit total crush while the viscous damper absorbs energy. The stiffness 𝐸2 prevents timestep problems. Both 𝐸1 and 𝑉2 are nonlinear with crush as follows: 𝑡 = 𝐸1(𝑉−n1), 𝐸1 𝑡 = 𝑉2(abs(1 − 𝑉)) 𝑉2 n2, (22.49.1) where 𝑉 is the relative volume defined by the ratio of the current to initial volume. Typical values are (units of N, mm, s) (22.49.2) 𝐸1 = 0.0036, 𝑛1 = 4.0, 𝑉2 = 0.0015, 𝐸2 = 100.0, 𝑛2 = 0.2, 𝜈 = 0.05. E1 V1 E2 Figure 22.49.1. Schematic of Material Model 62. LS-DYNA Theory Manual Material Models 22.50 Material Model 63: Crushable Foam The intent of this model is to model crushable foams in side impact and other applications where cyclic behavior is unimportant. This isotropic foam model crushes one-dimensionally with a Poisson’s ratio that is essentially zero. The stress versus strain behavior is depicted in Figure 22.50.1 where an example of unloading from point a to the tension cutoff stress at b then unloading to point c and finally reloading to point d is shown. At point d the reloading will continue along the loading curve. It is important to use nonzero values for the tension cutoff to prevent the disintegration of the material under small tensile loads. For high values of tension cutoff the behavior of the material will be similar in tension and compression. Viscous damping in the model follows an implementation identical to that of material type 57. In the implementation we assume that Young’s modulus is constant and update the stress assuming elastic behavior. trial = 𝜎𝑖𝑗 𝜎𝑖𝑗 𝑛 + 𝐸𝜀̇𝑖𝑗 𝑛+1 2⁄ Δ𝑡𝑛+1 2⁄ . (22.50.1) The magnitudes of the principal values, 𝜎𝑖 stress, 𝜎y, is exceeded and if so they are scaled back to the yield surface: trial, 𝑖 = 1,3 are then checked to see if the yield if 𝜎y < ∣𝜎𝑖 trial∣ then 𝜎𝑖 𝑛+1 = 𝜎y trial . trial∣ 𝜎𝑖 ∣σ𝑖 (22.50.2) After the principal values are scaled, the stress tensor is transformed back into ij Volumetric strain - In V Figure 22.50.1. Yield stress versus volumetric strain curve for the crushable foam. Material Models LS-DYNA Theory Manual the global system. As seen in Figure 22.50.1, the yield stress is a function of the natural logarithm of the relative volume, 𝑉, i.e., the volumetric strain. LS-DYNA Theory Manual Material Models 22.51 Material Model 64: Strain Rate Sensitive Power-Law Plasticity This material model follows a constitutive relationship of the form: 𝜎 = 𝑘𝜀𝑚𝜀̇𝑛 (22.51.1) where 𝜎 is the yield stress, 𝜀 is the effective plastic strain, 𝜀̇ is the effective plastic strain rate, and the constants 𝑘, 𝑚, and 𝑛 can be expressed as functions of effective plastic strain or can be constant with respect to the plastic strain. The case of no strain hardening can be obtained by setting the exponent of the plastic strain equal to a very small positive value, i.e., 0.0001. This model can be combined with the superplastic forming input to control the magnitude of the pressure in the pressure boundary conditions in order to limit the effective plastic strain rate so that it does not exceed a maximum value at any integration point within the model. A fully viscoplastic formulation is optional. An additional cost is incurred but the improvement in results can be dramatic. Material Models LS-DYNA Theory Manual 22.52 Material Model 65: Modified Zerilli/Armstrong The Armstrong-Zerilli Material Model expresses the flow stress as follows. For fcc metals, 𝜎 = C1 + {C2(𝜀p) 2⁄ [𝑒(−C3+C4ln(𝜀̇∗))𝑇] + C5} ( 𝜇(𝑇) 𝜇(293) ), (22.52.1) 𝜀p = effective plastic strain 𝜀̇∗ = 𝜀̇ 𝜀̇0 effective plastic strain rate where 𝜀̇0 = 1,1𝑒 − 3,1𝑒 − 6 for time units of seconds, milliseconds, and microseconds, respectively. For bcc metals, 𝜎 = C1 + C2𝑒(−C3+C4ln(𝜀̇∗))𝑇 + [C5(𝜀p)𝑛 + C6] ( 𝜇(𝑇) 𝜇(293) ), (22.52.2) where ( 𝜇(𝑇) 𝜇(293) ) = B1 + B2𝑇 + B3𝑇2. (22.52.3) The relationship between heat capacity (specific heat) and temperature may be characterized by a cubic polynomial equation as follows: Cp = G1 + G2𝑇 + G3𝑇2 + G4𝑇3. (22.52.4) A fully viscoplastic formulation is optional. An additional cost is incurred but the improvement in results can be dramatic. LS-DYNA Theory Manual Material Models 22.53 Material Model 66: Linear Stiffness/Linear Viscous 3D Discrete Beam The formulation of the discrete beam (Type 6) assumes that the beam is of zero length and requires no orientation node. A small distance between the nodes joined by the beam is permitted. The local coordinate system which determines (𝑟, 𝑠, 𝑡) is given by the coordinate ID in the cross sectional input where the global system is the default. The local coordinate system axes rotate with the average of the rotations of the two nodes that define the beam. For null stiffness coefficients, no forces corresponding to these null values will develop. The viscous damping coefficients are optional. Material Models LS-DYNA Theory Manual 22.54 Material Model 67: Nonlinear Stiffness/Viscous 3D Discrete Beam The formulation of the discrete beam (Type 6) assumes that the beam is of zero length and requires no orientation node. A small distance between the nodes joined by the beam is permitted. The local coordinate system which determines (𝑟, 𝑠, 𝑡) is given by the coordinate ID in the cross sectional input where the global system is the default. The local coordinate system axes rotate with the average of the rotations of the two nodes that define the beam. For null load curve ID’s, no forces are computed. The force resultants are found from load curves that are defined in terms of the force resultant versus the relative displacement in the local coordinate system for the discrete beam. (b.) (a.) DISPLACEMENT Figure 22.54.1. The resultant forces and moments are determined by a table lookup. If the origin of the load curve is at [0,0] as in (b.) and tension and compression responses are symmetric. |DISPLACEMENT| LS-DYNA Theory Manual Material Models 22.55 Material Model 68: Nonlinear Plastic/Linear Viscous 3D Discrete Beam The formulation of the discrete beam (Type 6) assumes that the beam is of zero length and requires no orientation node. A small distance between the nodes joined by the beam is permitted. The local coordinate system which determines (𝑟, 𝑠, 𝑡) is given by the coordinate ID in the cross sectional input where the global system is the default. The local coordinate system axes rotate with the average of the rotations of the two nodes that define the beam. Each force resultant in the local system can have a limiting value defined as a function of plastic displacement by using a load curve . For the degrees of freedom where elastic behavior is desired, the load curve ID is simply set to zero. Catastrophic failure, based on force resultants, occurs if the following inequality is satisfied: ( 𝐹r fail 𝐹r ) + ( 𝐹s fail 𝐹s ) + ( 𝐹t fail 𝐹t ) + ( 𝑀r fail 𝑀r ) + ( 𝑀s fail 𝑀s ) + ( 𝑀t fail 𝑀t ) − 1. ≥ 0. (22.55.1) Likewise, catastrophic failure based on displacement resultants occurs if: ( 𝑢r fail 𝑢r ) + ( 𝑢s fail 𝑢s ) + ( 𝑢t fail 𝑢t ) + ( 𝜃r fail 𝜃r ) + ( 𝜃s fail 𝜃s ) + ( 𝜃t fail 𝜃t ) − 1. ≥ 0. (22.55.2) After failure, the discrete element is deleted. If failure is included, either one or both of the criteria may be used. PLASTIC DISPLACEMENT Figure 22.55.1. The resultant forces and moments are limited by the yield definition. The initial yield point corresponds to a plastic displacement of zero. Material Models LS-DYNA Theory Manual 22.56 Material Model 69: Side Impact Dummy Damper (SID Damper) The side impact dummy uses a damper that is not adequately treated by nonlinear force versus relative velocity curves, since the force characteristics are also dependent on the displacement of the piston. As the damper moves, the fluid flows through the open orifices to provide the necessary damping resistance. While moving as shown in Figure 22.56.1, the piston gradually blocks off and effectively closes the orifices. The number of orifices and the size of their openings control the damper resistance and performance. The damping force is computed from the equation: 𝐹 = 𝑆𝐹 {⎧ ⎩{⎨ 𝐾𝐴p𝑉p {⎧𝐶1 ⎩{⎨ 𝐴0 𝑡 + 𝐶2∣𝐕p∣𝜌fluid 𝐴p 𝐶𝐴0 𝑡 ) ⎡( ⎢ ⎣ − 1 }⎫ ⎭}⎬ ⎤ ⎥ ⎦ }⎫ − 𝑓 (𝑠 + 𝑠0) + 𝑉p𝑔(𝑠 + 𝑠0) ⎭}⎬ , (22.56.1) where 𝐾 is a user defined constant or a tabulated function of the absolute value of the relative velocity, 𝐕p is the piston's relative velocity, 𝐶 is the discharge coefficient, 𝐴p is 𝑡 is the total open areas of orifices at time 𝑡, 𝜌fluid is the fluid density, the piston area, 𝐴0 𝐶1 is the coefficient for the linear term, and 𝐶2 is the coefficient for the quadratic term. d4 d3 d2 d1 Piston Vp ith Piston Orifice Orifice Opening Controller Figure 22.56.1. Mathematical model for the Side Impact Dummy damper. 2Ri - h LS-DYNA Theory Manual Material Models Last orifice closes. Force increases as orifice is gradually covered. DISPLACEMENT Figure 22.56.2. Force versus displacement as orifices are covered at a constant relative velocity. Only the linear velocity term is active. In the implementation, the orifices are assumed to be circular with partial covering by the orifice controller. As the piston closes, the closure of the orifice is gradual. This gradual closure is taken into account to insure a smooth response. If the piston stroke is exceeded, the stiffness value, 𝑘, limits further movement, i.e., if the damper bottoms out in tension or compression, the damper forces are calculated by replacing the damper by a bottoming out spring and damper, k and c, respectively. The piston stroke must exceed the initial length of the beam element. The time step calculation is based in part on the stiffness value of the bottoming out spring. A typical force versus displacement curve at constant relative velocity is shown in Figure 22.56.2. The factor, SF, which scales the force defaults to 1.0 and is analogous to the adjusting ring on the damper. Material Models LS-DYNA Theory Manual 22.57 Material Model 70: Hydraulic/Gas Damper This special purpose element represents a combined hydraulic and gas-filled damper which has a variable orifice coefficient. A schematic of the damper is shown in Figure 22.57.1. Dampers of this type are sometimes used on buffers at the end of railroad tracks and as aircraft undercarriage shock absorbers. This material can be used only as a discrete beam element. As the damper is compressed two actions contribute to the force that develops. First, the gas is adiabatically compressed into a smaller volume. Secondly, oil is forced through an orifice. A profiled pin may occupy some of the cross-sectional area of the orifice; thus, the orifice area available for the oil varies with the stroke. The force is assumed proportional to the square of the velocity and inversely proportional to the available area. The equation for this element is: 𝐹 = SCLF ⋅ {𝐾h ( 𝑎0 ) + [𝑃0 ( 𝐶0 𝐶0 − 𝑆 ) − 𝑃a] ⋅ 𝐴p}, (22.57.1) where 𝑆 is the element deflection and 𝑉 is the relative velocity across the element. Orifice Oil Profiled Pin Gas Figure 22.57.1. Schematic of Hydraulic/Gas damper. LS-DYNA Theory Manual Material Models 22.58 Material Model 71: Cable This material can be used only as a discrete beam element. The force, 𝐹, generated by the cable is nonzero only if the cable is in tension. The force is given by: 𝐹 = 𝐾 ⋅ max(Δ𝐿, 0. ), (22.58.1) where Δ𝐿 is the change in length Δ𝐿 = current length − (initial length-offset), (22.58.2) and the stiffness is defined as: 𝐾 = 𝐸 ⋅ area (initial length- offset) . (22.58.3) The area and offset are defined on either the cross section or element cards in the LS-DYNA input. For a slack cable the offset should be input as a negative length. For an initial tensile force the offset should be positive. If a load curve is specified, the Young’s modulus will be ignored and the load curve will be used instead. The points on the load curve are defined as engineering stress versus engineering strain, i.e., the change in length over the initial length. The unloading behavior follows the loading. Material Models LS-DYNA Theory Manual 22.59 Material Model 73: Low Density Viscoelastic Foam This viscoelastic foam model is available to model highly compressible viscous foams. The hyperelastic formulation of this model follows that of material 57. Rate effects are accounted for through linear viscoelasticity by a convolution integral of the form r = ∫ 𝑔𝑖𝑗𝑘𝑙 𝜎𝑖𝑗 where 𝑔𝑖𝑗𝑘𝑙(𝑡 − 𝜏) is the relaxation function. The stress tensor, 𝜎𝑖𝑗 determined from the foam, 𝜎𝑖𝑗 summation of the two contributions: (𝑡 − 𝜏) r , augments the stresses f ; consequently, the final stress, 𝜎𝑖𝑗, is taken as the (22.59.1) 𝑑𝜏, 𝜕𝜀𝑘𝑙 𝜕𝜏 𝜎𝑖𝑗 = 𝜎𝑖𝑗 r . f + 𝜎𝑖𝑗 (22.59.2) Since we wish to include only simple rate effects, the relaxation function is represented by up to six terms of the Prony series: 𝑔(𝑡) = 𝛼0 + ∑ 𝛼𝑚 𝑚=1 𝑒−𝛽𝑡. (22.59.3) This model is effectively a Maxwell fluid which consists of a dampers and springs in series. The formulation is performed in the local system of principal stretches where only the principal values of stress are computed and triaxial coupling is avoided. Consequently, the one-dimensional nature of this foam material is unaffected by this addition of rate effects. The addition of rate effects necessitates 42 additional history variables per integration point. The cost and memory overhead of this model comes primarily from the need to “remember” the local system of principal stretches and the evaluation of the viscous stress components. Viscous damping in the model follows an implementation identical to that of material type 57. LS-DYNA Theory Manual Material Models 22.60 Material Model 74: Elastic Spring for the Discrete Beam This model permits elastic springs with damping to be combined and represented with a discrete beam element type 6. Linear stiffness and damping coefficients can be defined, and, for nonlinear behavior, a force versus deflection and force versus rate curves can be used. Displacement based failure and an initial force are optional. If the linear spring stiffness is used, the force, F, is given by: where K is the stiffness constant, and D is the viscous damping coefficient. 𝐹 = 𝐹0 + 𝐾Δ𝐿 + 𝐷Δ𝐿̇, (22.60.1) If the load curve ID for 𝑓 (Δ𝐿) is specified, nonlinear behavior is activated. For this case the force is given by: 𝐹 = 𝐹0 + 𝐾 𝑓 (Δ𝐿) [1 + C1 ⋅ Δ𝐿̇ + C2 ⋅ sgn(Δ𝐿̇)ln (max {1. , ∣Δ𝐿̇∣ DLE })] (22.60.2) +𝐷Δ𝐿̇ + 𝑔(Δ𝐿)ℎ(Δ𝐿̇), where C1 and C2 are damping coefficients for nonlinear behavior, DLE is a factor to scale time units, and 𝑔(Δ𝐿) is an optional load curve defining a scale factor versus deflection for load curve ID, ℎ(𝑑Δ𝐿/𝑑𝑡). In these equations, Δ𝐿 is the change in length Δ𝐿 = current length-initial length. (22.60.3) Failure can occur in either compression or tension based on displacement values of CDF and TDF, respectively. After failure no forces are carried. Compressive failure does not apply if the spring is initially zero length. The cross sectional area is defined on the section card for the discrete beam elements, in *SECTION_BEAM. The square root of this area is used as the contact thickness offset if these elements are included in the contact treatment. Material Models LS-DYNA Theory Manual 22.61 Material Model 75: Bilkhu/Dubois Foam Model This model uses uniaxial and triaxial test data to provide a more realistic treatment of crushable foam. The Poisson’s ratio is set to zero for the elastic response. The volumetric strain is defined in terms of the relative volume, 𝑉, as: 𝛾 = −ln(𝑉). (22.61.1) In defining the curves, the stress and strain pairs should be positive values starting with a volumetric strain value of zero. Viscous damping in the model follows an implementation identical to that of material type 57. Uniaxial Yield Stress Pressure Yield Figure 22.61.1. Behavior of crushable foam. Unloading is elastic. Volumetric Strain LS-DYNA Theory Manual Material Models 22.62 Material Model 76: General Viscoelastic 22.62.1 Introduction Material type 76 in LS-DYNA is a general viscoelastic Maxwell model having up to 18 terms in the prony series expansion and is useful for modeling dense continuum rubbers and solid explosives. It is characterized in the input by bulk and shear modulii, 𝑔 . Either the coefficients of the 𝐾𝑚 and 𝐺𝑚, and associated decay constants, 𝛽𝑚 prony series expansion can be used directly, or a relaxation curve may be specified to define the viscoelastic deviatoric and bulk behavior. 𝑘 and 𝛽𝑚 22.62.2 Constitutive Model The model is a hypoelastic version of the model given by Christensen and can be stated as 𝝈∇ = ∑(𝐾𝑚𝑡𝑚 ∇ ) ∇ 𝒊 + 2𝐺𝑚𝒔𝑚 , (22.62.1) where 𝑡𝑚 and 𝒔𝑚 are (strain) quantities governed by the following evolution in time ∇ = 𝑫dev − 𝛽𝑚 𝒔𝑚 𝑔 𝒔𝑚 (22.62.2) and 𝑘 𝑡𝑚 ∇ = 𝐷vol − 𝛽𝑚 𝑡𝑚 (22.62.3) 𝑔 are the Here 𝐾𝑚 and 𝐺𝑚 are bulk and shear moduli, respectively, 𝛽𝑚 corresponding decay coefficients, 𝐷vol and 𝑫dev are the volumetric and deviatoric strain rates, 𝒊 is the 2nd order identity tensor and ∇ denotes the Jaumann objective rate. It should immediately be noted that for all decay coefficients equal to 0 (zero), the model is reduced to a time independent elastic model, 𝑘 and 𝛽𝑚 𝝈 ∇ = 𝐾𝐷vol𝒊 + 2𝐺𝑫dev with bulk and shear modulus given by 𝐾 = ∑ 𝐾𝑚𝑚 displacement theory, the stress can be integrated to be given by and 𝐺 = ∑ 𝐺𝑚𝑚 (22.62.4) . For small 𝝈(𝑡) = ∑ (𝐾𝑚 ∫ 𝑒−𝛽𝑚 𝑘 (𝑡−𝜏)𝐷vol(𝜏) 𝑑𝜏𝒊 + 2𝐺𝑚 ∫ 𝑒−𝛽𝑚 𝑔 (𝑡−𝜏)𝑫dev(𝜏) 𝑑𝜏) (22.62.5) For shell elements, the same theory applies except that the objective rate ∇ is the corotational time derivative instead of the Jaumann rate. 22.62.3 Tangent Modulus For the implicit tangent modulus, we note that the internal force contribution depends on the displacement and time, which we denote 𝒇int = 𝒇int(𝒖, 𝑡). The time derivative of this vector is the sum of a material and a geometric contribution. The material contribution is given by Material Models LS-DYNA Theory Manual Stress relaxation curve 10n 10n+1 10n+2 time Optional ramp time for loading load curve should be equally spaced on the Figure 22.62.1. Relaxation curve. This curve defines stress versus time where time is defined on a logarithmic scale. For best results, the points defined in the logarithmic scale. Furthermore, the load curve should be smooth and defined in the positive quadrant. If nonphysical values are determined by least squares fit, LS-DYNA will terminate with an error message after the initialization phase is completed. If the ramp time for loading is included, then the relaxation which occurs during the loading phase is taken into account. This effect may or may not be important. 𝒇 ̇ mat = ∫ 𝑩𝑇 𝝈 ∇𝑇𝑑Ω int (22.62.6) where 𝑩 is the strain displacement matrix, the integration is over the current configuration Ω and ∇𝑇 stands for Truesdell rate. This expression should later be identified with 𝒇 ̇ mat = int mat 𝜕𝒇int 𝜕𝒖 𝒖̇ + mat 𝜕𝒇int 𝜕𝑡 (22.62.7) in order to determine the tangent modulus. Neglecting discrepancies between the Jaumann and Truesdell rates, we can use (22.62.2) and (22.62.3) in (22.62.6) to get 𝒇 ̇ mat = ∫ 𝑩𝑇 ∑(𝐾𝑚𝒊⨂𝒊 + 2𝐺𝑚𝑰dev) int 𝑩𝑑𝛺 𝒖̇ − ∫ 𝑩𝑇 ∑(𝐾𝑚𝛽𝑚 𝑘 𝑡𝑚𝒊 + 2𝐺𝑚𝛽𝑚 𝑔 𝒔𝑚) 𝑑𝛺, (22.62.8) where 𝑰dev is the 4th order deviatoric identity tensor. Comparing this expression with (22.62.7) one can conclude that mat 𝜕𝒇int 𝜕𝒖 = ∫ 𝑩𝑇 ∑(𝐾𝑚𝒊⨂𝒊 + 2𝐺𝑚𝑰dev) 𝑩𝑑𝛺, and hence the tangent modulus is 22-162 (Material Models) LS-DYNA Theory Manual Material Models . 𝑪 = ∑(𝐾𝑚𝒊⨂𝒊 + 2𝐺𝑚𝑰dev) (22.62.10) i.e., independent of deformation and time. In fact, this tangent modulus is equal to the classical elastic tangent modulus for a hypoelastic material, cf. (22.62.4). 22.62.4 Using the Relaxation Curve Instead of inputting the stiffness and relaxation parameters, one can input a relaxation curve from test according to Figure 22.62.1. The time scale is determined by BSTART and LS-DYNA will determine all parameters as to best fit the curve. Material Models LS-DYNA Theory Manual 22.63 Material Model 77: Hyperviscoelastic Rubber Material type 77 in LS-DYNA consists of two hyperelastic rubber models, a general hyperelastic rubber model and an Ogden rubber model, that can be combined optionally with a viscoelastic stress contribution. As for the rate independent part, the constitutive law is determined by a strain energy function which in this case advantageously can be expressed in terms of the principal stretches, i.e., 𝑊 = 𝑊(𝜆1, 𝜆2, 𝜆3). To obtain the Cauchy stress 𝜎𝑖𝑗, as well as the constitutive tensor of TC, they are first calculated in the principal basis after which they are interest, 𝐷𝑖𝑗𝑘𝑙 transformed back to the “base frame”, or standard basis. The complete set of formulas is given by Crisfield [1997] and is for the sake of completeness recapitulated here. The principal Kirchoff stress components are given by E = 𝜆𝑖 𝜏𝑖𝑖 𝜕𝑊 𝜕𝜆𝑖 (no sum), that are transformed to the standard basis using the standard formula E. 𝜏𝑖𝑗 = 𝑞𝑖𝑘𝑞𝑗𝑙𝜏𝑘𝑙 (22.63.1) (22.63.2) The 𝑞𝑖𝑗 are the components of the orthogonal tensor containing the eigenvectors of the principal basis. The Cauchy stress is then given by 𝜎𝑖𝑗 = 𝐽−1𝜏𝑖𝑗, (22.63.3) where 𝐽 = 𝜆1𝜆2𝜆3 is the relative volume change. The constitutive tensor that relates the rate of deformation to the Truesdell (convected) rate of Kirchoff stress can in the principal basis be expressed as 𝐷𝑖𝑖𝑗𝑗 TKE = 𝜆𝑗 TKE = 𝐷𝑖𝑗𝑖𝑗 TKE = 𝐷𝑖𝑗𝑖𝑗 E𝛿𝑖𝑗 − 2𝜏𝑖𝑖 𝜕𝜏𝑖𝑖 𝜕𝜆𝑗 2𝜏𝑗𝑗 E − 𝜆𝑖 2𝜏𝑖𝑖 𝜆𝑗 2 − 𝜆𝑗 𝜆𝑖 𝜕𝜏𝑖𝑖 ( 𝜕𝜆𝑖 𝜆𝑖 − 𝜕𝜏𝑖𝑖 𝜕𝜆𝑗 ), 𝑖 ≠ 𝑗, 𝜆𝑖 = 𝜆𝑗 , 𝑖 ≠ 𝑗, 𝜆𝑖 ≠ 𝜆𝑗 (no sum). (22.63.4) These components are transformed to the standard basis according to TK = 𝑞𝑖𝑝𝑞𝑗𝑞𝑞𝑘𝑟𝑞𝑙𝑠𝐷𝑝𝑞𝑟𝑠 TKE, 𝐷𝑖𝑗𝑘𝑙 (22.63.5) and finally the constitutive tensor relating the rate of deformation to the Truesdell rate of Cauchy stress is obtained through LS-DYNA Theory Manual Material Models 𝐷𝑖𝑗𝑘𝑙 TC = 𝐽−1𝐷𝑖𝑗𝑘𝑙 TK . (22.63.6) When dealing with shell elements, the tangent moduli in the corotational coordinates is of interest. This matrix is given by 𝐷̂ TC = 𝑅𝑝𝑖𝑅𝑞𝑗𝑅𝑟𝑘𝑅𝑠𝑙𝐷𝑝𝑞𝑟𝑠 𝑖𝑗𝑘𝑙 TC = 𝐽−1𝑅𝑝𝑖𝑅𝑞𝑗𝑅𝑟𝑘𝑅𝑠𝑙𝐷𝑝𝑞𝑟𝑠 TK = 𝐽−1𝑞 ̂𝑖𝑝𝑞 ̂𝑗𝑞𝑞 ̂𝑘𝑟𝑞 ̂𝑙𝑠𝐷𝑝𝑞𝑟𝑠 TKE, (22.63.7) where 𝑅𝑖𝑗 is the matrix containing the unit basis vectors of the corotational system and 𝑞 ̂𝑖𝑗 = 𝑅𝑘𝑖𝑞𝑘𝑗. The latter matrix can be determined as the eigenvectors of the co-rotated left Cauchy-Green tensor (or the left stretch tensor). In LS-DYNA, the tangent stiffness matrix is after assembly transformed back to the standard basis according to standard transformation formulae. 22.63.1 General Hyperelastic Rubber Model The strain energy function for the general hyperelastic rubber model is given by 𝑊 = ∑ 𝐶𝑝𝑞𝑊1 𝑝,𝑞=0 𝑝𝑊2 + 𝐾(𝐽 − 1)2, where 𝐾 is the bulk modulus, −1 3 − 3 𝑊1 = 𝐼1𝐼3 −2/3 − 3, 𝑊2 = 𝐼2𝐼3 and 𝐼1 = 𝜆1 𝐼2 = 𝜆1 𝐼3 = 𝜆1 2 + 𝜆2 2𝜆2 2𝜆2 2 + 𝜆2 2, 2𝜆3 2 + 𝜆3 2 + 𝜆1 2𝜆3 2 2𝜆3 (22.63.8) (22.63.9) (22.63.10) are the invariants in terms of the principal stretches. To apply the formulas in the previous section, we require E = 𝜆𝑖 𝜏𝑖𝑖 𝜕𝑊 𝜕𝜆𝑖 where = ∑ 𝐶𝑝𝑞(𝑝𝑊1 𝑝−1𝑊1𝑖 ′ 𝑊2 𝑞 + 𝑞𝑊1 𝑝𝑊2 𝑞−1𝑊2𝑖 ′ ) + 𝐾𝐽(𝐽 − 1), (22.63.11) 𝑝,𝑞=0 𝑊1𝑖 ′ ≔ 𝜆𝑖 𝑊2𝑖 ′ : = 𝜆𝑖 𝜕𝑊1 𝜕𝜆𝑖 𝜕𝑊2 𝜕𝜆𝑖 = (2𝜆𝑖 2 − −1 𝐼1) 𝐼3 = (2𝜆𝑖 2(𝐼1 − 𝜆𝑖 2) − −2 3. 𝐼2) 𝐼3 (22.63.12) If C𝑝𝑞 is nonzero only for 𝑝𝑞 = 01,10,11,20,02,30, then Equation (22.63.11) can be written as Material Models LS-DYNA Theory Manual E = (𝐶10 + 𝐶11𝑊2 + 2𝐶20𝑊1 + 3𝐶30𝑊1 𝜏𝑖𝑖 (𝐶01 + 𝐶11𝑊1 + 2𝐶02𝑊2)𝑊2𝑖 ′ + 2)𝑊1𝑖 ′ + 𝐾𝐽(𝐽 − 1). (22.63.13) Proceeding with the constitutive tensor, we have 𝜆𝑗 𝜕𝜏𝑖𝑖 𝜕𝜆𝑗 𝑝,𝑞=0 = ∑ 𝐶𝑝𝑞(𝑝(𝑝 − 1)𝑊1 𝑝−2𝑊1𝑖 ′ 𝑊1𝑗 ′ 𝑊2 𝑞 + 𝑝𝑊1 𝑝−1𝑊1𝑖𝑗 ′′ 𝑊2 𝑞 + 𝑝𝑞𝑊1 𝑝−1𝑊1𝑖 ′ 𝑊2 𝑞−1𝑊2𝑗 ′ 𝑝−1𝑊1𝑗 +𝑞𝑝𝑊1 +𝐾𝐽(2𝐽 − 1), ′ 𝑊2 𝑞−1𝑊2𝑖 ′ + 𝑞(𝑞 − 1)𝑊1 𝑝𝑊2 𝑞−2𝑊2𝑖 ′ 𝑊2𝑗 ′ + 𝑞𝑊1 𝑝𝑊2 𝑞−1𝑊2𝑖𝑗 ′′ ) where 𝑊1𝑖𝑗 ′′ : = 𝜆𝑗 𝑊2𝑖𝑗 ′′ : = 𝜆𝑗 ′ 𝜕𝑊1𝑖 𝜕𝜆𝑗 ′ 𝜕𝑊2𝑖 𝜕𝜆𝑗 = (4𝜆𝑖 2𝛿𝑖𝑗 − (𝜆𝑖 2 + 𝜆𝑗 2) + −1/3 𝐼1)𝐼3 = ((4𝜆𝑖 2𝐼1 − 8𝜆𝑖 4)𝛿𝑖𝑗 + 4𝜆𝑖 2𝜆𝑗 2 − (𝜆𝑖 2(𝐼1 − 𝜆𝑖 2) + 𝜆𝑗 2(𝐼1 − 𝜆𝑗 2)) + (22.63.14) (22.63.15) 16 −2/3 𝐼2)𝐼3 Again, using only the nonzero coefficients mentioned above, Equation (22.63.14) is reduced to 𝜆𝑗 𝜕𝜏𝑖𝑖 𝜕𝜆𝑗 = 𝐶11(𝑊1𝑖 ′ 𝑊2𝑗 ′ + 𝑊1𝑗 ′ 𝑊2𝑖 ′ ) + 2(𝐶20 + 3𝐶30𝑊1)𝑊1𝑗 ′ 𝑊1𝑖 ′ + 2𝐶02𝑊2𝑖 ′ 𝑊2𝑗 ′ + (𝐶10 + 𝐶11𝑊2 + 2𝐶20𝑊1 + 3𝐶30𝑊1 𝐾𝐽(2𝐽 − 1). 2)𝑊1𝑖𝑗 ′′ + (𝐶01 + 𝐶11𝑊1 + 2𝐶02𝑊2)𝑊2𝑖𝑗 ′′ + 22.63.2 Ogden Rubber Model The strain energy function for the Ogden rubber model is given by 𝑊 = ∑ 𝑚=1 𝜇𝑚 𝛼𝑚 (𝜆̃ 𝛼𝑚 + 𝜆̃ 𝛼𝑚 + 𝜆̃ 𝛼𝑚 − 3) + 𝐾(𝐽 − 1)2, where 𝜆̃𝑖 = 𝜆𝑖 𝐽1/3, (22.63.16) (22.63.17) (22.63.18) are the volumetric independent principal stretches, and 𝜇𝑚 and 𝛼𝑚 are material parameters. To apply the formulas in the previous section, we require E = 𝜆𝑖 𝜏𝑖𝑖 𝜕𝑊 𝜕𝜆𝑖 = ∑ 𝜇𝑚(𝜆̃ 𝑚=1 𝛼𝑚 − 𝑎𝑚) + 𝐾𝐽(𝐽 − 1), (22.63.19) where 22-166 (Material Models) 𝑎𝑚 = 𝜆̃ 𝛼𝑚 + 𝜆̃ 𝛼𝑚 + 𝜆̃ 𝛼𝑚. LS-DYNA Theory Manual Material Models Proceeding with the constitutive tensor, we have 𝜆𝑗 𝜕𝜏𝑖𝑖 𝜕𝜆𝑗 = ∑ 𝑚=1 𝜇𝑚𝛼𝑚 ( 𝑎𝑚 + 3𝜆̃ 𝛼𝑚𝛿𝑖𝑗 − 𝜆̃ 𝛼𝑚 − 𝜆̃ 𝛼𝑚) + 𝐾𝐽(2𝐽 − 1). (22.63.21) 22.63.3 The Viscoelastic Contribution As mentioned above, this material model is accompanied with a viscoelastic stress contribution. The rate form of this constitutive law can in co-rotational coordinates be written • ve 𝜎̂𝑖𝑗 = ∑ 2𝐺𝑚 𝑚=1 𝐷̂ 𝑖𝑗 dev − ∑ 2𝛽𝑚𝐺𝑚 ∫ 𝑒−𝛽𝑚(𝑡−𝜏)𝐷̂ 𝑖𝑗 dev(𝜏)𝑑𝜏 . (22.63.22) 𝑚=1 Here 𝑛 is a number less than or equal to 6, 𝜎̂𝑖𝑗 ve is the co-rotated viscoelastic stress, dev is the deviatoric co-rotated rate-of-deformation and 𝐺𝑚 and 𝛽𝑚 are material 𝐷̂ 𝑖𝑗 parameters. The parameters 𝐺𝑚 can be thought of as shear moduli and 𝛽𝑚 as decay coefficients determining the relaxation properties of the material. This rate form can be integrated in time to form the corotated viscoelastic stress ve = ∑ 2𝐺𝑚 ∫ 𝑒−𝛽𝑚(𝑡−𝜏)𝐷̂ 𝑖𝑗 𝜎̂𝑖𝑗 𝑚=1 dev(𝜏)𝑑𝜏 . (22.63.23) For the constitutive matrix, we refer to Borrvall [2002] and here simply state that it is equal to 𝐷̂ TCve = ∑ 2𝐺𝑚 𝑖𝑗𝑘𝑙 𝑚=1 ( (𝛿𝑖𝑘𝛿𝑗𝑙 + 𝛿𝑖𝑙𝛿𝑗𝑘) − 𝛿𝑖𝑗𝛿𝑘𝑙). (22.63.24) 22.63.4 Stress Update for Shell Elements In principal, the stress update for material 77 and shell elements follows closely the one that is implemented for material 27. The stress is evaluated in corotational coordinates after which it is transformed back to the standard basis according to 𝜎𝑖𝑗 = 𝑅𝑖𝑘𝑅𝑗𝑙𝜎̂𝑘𝑙, (22.63.25) or equivalently the internal force is assembled in the corotational system and then transformed back to the standard basis according to standard transformation formulae. Here 𝑅𝑖𝑗 is the rotation matrix containing the corotational basis vectors. The so-called Material Models LS-DYNA Theory Manual corotated stress 𝜎̂𝑖𝑗 is evaluated as the sum of the stresses given in Sections 19.77.1 and 19.77.4. The viscoelastic stress contribution is incrementally updated with aid of the corotated rate of deformation. To be somewhat more precise, the values of the 12 integrals in Equation (22.63.23) are kept as history variables that are updated in each time step. Each integral is discretized in time and the mean value theorem is used in each time step to determine their values. For the hyperelastic stress contribution, the principal stretches are needed and here taken as the square root of the eigenvalues of the co-rotated left Cauchy-Green tensor 𝑏̂ 𝑖𝑗. The corotated left Cauchy-Green tensor is incrementally updated with the aid of a time increment Δ𝑡, the corotated velocity gradient 𝐿̂ 𝑖𝑗, and the angular velocity 𝛺̂𝑖𝑗 with which the embedded coordinate system is rotating, 𝑖𝑗 = 𝑏̂ 𝑏̂ 𝑖𝑗 + Δ𝑡(𝐿̂ 𝑖𝑘 − 𝛺̂𝑖𝑘)𝑏̂ 𝑘𝑗 + Δ𝑡𝑏̂ 𝑖𝑘(𝐿̂ 𝑖𝑘 − 𝛺̂𝑖𝑘). (22.63.26) The primary reason for taking a corotational approach is to facilitate the maintenance of a vanishing normal stress through the thickness of the shell, something that is achieved by adjusting the corresponding component of the corotated velocity gradient 𝐿̂ 33 accordingly. The problem can be stated as to determine L̂ 33 such that when updating the left Cauchy-Green tensor through Equation (22.63.26) and subsequently the stress through formulae in Sections 19.77.1 and 19.77.4, 𝜎̂33 = 0. To this end, it is assumed that 𝐿̂ 33 = α(𝐿̂ 11 + 𝐿̂ 22), (22.63.27) for some parameter α that is determined in the following three step procedure. In the (0) first two steps, α = 0 and α = −1, respectively, resulting in two trial normal stresses 𝜎̂33 (−1). Then it is assumed that the actual normal stress depends linearly on α, and 𝜎̂33 meaning that the latter can be determined from 0 = 𝜎33 (α) = 𝜎33 (0) + α(𝜎33 (0) − 𝜎33 (−1)). In the current implementation, α is given by (0) 𝜎̂33 (−1) − 𝜎̂33 𝜎̂33 (0) if ∣𝜎̂33 (−1) − 𝜎̂33 (0)∣ ≥ 10−4 − 1 otherwise 𝛼 = ⎧ { { { ⎨ { { { ⎩ (22.63.28) (22.63.29) and the stresses are determined from this value of 𝛼. Finally, to make sure that the normal stress through the thickness vanishes, it is set to 0 (zero) before exiting the stress update routine. LS-DYNA Theory Manual Material Models 22.64 Material Model 78: Soil/Concrete Concrete pressure is positive in compression. Volumetric strain is defined as the natural log of the relative volume and is positive in compression where the relative volume, 𝑉, is the ratio of the current volume to the initial volume. The tabulated data should be given in order of increasing compression. If the pressure drops below the cutoff value specified, it is reset to that value and the deviatoric stress state is eliminated. If the load curve ID is provided as a positive number, the deviatoric perfectly plastic pressure dependent yield function 𝜙, is described in terms of the second invariant, 𝐽2, the pressure, 𝑝, and the tabulated load curve, 𝐹(𝑝), as 𝜙 = √3𝐽2 − 𝐹(𝑝) = σ𝑦 − 𝐹(𝑝), where 𝐽2 is defined in terms of the deviatoric stress tensor as: assuming that if the ID is given as negative, then the yield function becomes: 𝑆𝑖𝑗𝑆𝑖𝑗, 𝐽2 = being the deviatoric stress tensor. 𝜙 = 𝐽2 − 𝐹(𝑝), (22.64.1) (22.64.2) (22.64.3) If cracking is invoked, the yield stress is multiplied by a factor f which reduces with plastic stain according to a trilinear law as shown in Figure 22.64.1. 1.0 Figure 22.64.1. Strength reduction factor. Material Models LS-DYNA Theory Manual Figure 22.64.2. Cracking strain versus pressure. b = residual strength factor 𝜀1 = plastic stain at which cracking begins. 𝜀2 = plastic stain at which residual strength is reached. 𝜀1 and 𝜀2 are tabulated functions of pressure that are defined by load curves . The values on the curves are pressure versus strain and should be entered in order of increasing pressure. The strain values should always increase monotonically with pressure. By properly defining the load curves, it is possible to obtain the desired strength and ductility over a range of pressures. See Figure 22.64.3. Yield stress p3 p2 p1 Plastic strain Figure 22.64.3. Example Caption LS-DYNA Theory Manual Material Models 22.65 Material Model 79: Hysteretic Soil This model is a nested surface model with five superposed “layers” of elasto- perfectly plastic material, each with its own elastic modulii and yield values. Nested surface models give hysteretic behavior, as the different “layers” yield at different stresses. The constants 𝑎0, 𝑎1, 𝑎2 govern the pressure sensitivity of the yield stress. Only the ratios between these values are important - the absolute stress values are taken from the stress-strain curve. The stress strain pairs (𝛾1, 𝜏1), ... (𝛾5, 𝜏5) define a shear stress versus shear strain curve. The first point on the curve is assumed by default to be (0,0) and does not need to be entered. The slope of the curve must decrease with increasing 𝛾. Not all five points need be to be defined. This curve applies at the reference pressure; at other pressures the curve varies according to 𝑎0, 𝑎1, and 𝑎2 as in the soil and crushable foam model, Material 5. The elastic moduli 𝐺 and 𝐾 are pressure sensitive. 𝐺 = 𝐺0(𝑝 − 𝑝0)𝑏, 𝐾 = 𝐾0(𝑝 − 𝑝0)𝑏, (22.65.1) where 𝐺0 and 𝐾0 are the input values, 𝑝 is the current pressure, 𝑝0 the cut-off or reference pressure (must be zero or negative). If 𝑝 attempts to fall below 𝑝0 (i.e., more tensile) the shear stresses are set to zero and the pressure is set to 𝑝0. Thus, the material has no stiffness or strength in tension. The pressure in compression is calculated as follows: where 𝑉 is the relative volume, i.e., the ratio between the original and current volume. 𝑝 = [−𝐾0ln(𝑉)] 1−𝑏⁄ , (22.65.2) Material Models LS-DYNA Theory Manual 22.66 Material Model 80: Ramberg-Osgood Plasticity The Ramberg-Osgood equation is an empirical constitutive relation to represent the one-dimensional elastic-plastic behavior of many materials, including soils. This model allows a simple rate independent representation of the hysteretic energy dissipation observed in soils subjected to cyclic shear deformation. For monotonic loading, the stress-strain relationship is given by: 𝛾𝑦 𝛾𝑦 = = 𝜏𝑦 𝜏𝑦 + 𝛼 ∣ − 𝛼 ∣ 𝜏𝑦 𝜏𝑦 ∣ ∣ if 𝛾 ≥ 0, if 𝛾 < 0, (22.66.1) where 𝛾 is the shear and 𝜏 is the stress. The model approaches perfect plasticity as the stress exponent 𝑟 → ∞. These equations must be augmented to correctly model unloading and reloading material behavior. The first load reversal is detected by 𝛾𝛾̇ < 0. After the first reversal, the stress-strain relationship is modified to (𝛾 − 𝛾0) 2𝛾𝑦 (𝛾 − 𝛾0) 2𝛾𝑦 = = (𝜏 − 𝜏0) 2𝜏𝑦 (𝜏 − 𝜏0) 2𝜏𝑦 + 𝛼 ∣ − 𝛼 ∣ (𝜏 − 𝜏0) ∣ 2𝜏𝑦 (𝜏 − 𝜏0) ∣ 2𝜏𝑦 if 𝛾 ≥ 0, if 𝛾 < 0, (22.66.2) where 𝛾0 and 𝜏0 represent the values of strain and stress at the point of load reversal. Subsequent load reversals are detected by (𝛾 − 𝛾0)𝛾̇ < 0. The Ramberg-Osgood equations are inherently one-dimensional and are assumed to apply to shear components. To generalize this theory to the multidimen- sional case, it is assumed that each component of the deviatoric stress and deviatoric tensorial strain is independently related by the one-dimensional stress-strain equations. A projection is used to map the result back into deviatoric stress space if required. The volumetric behavior is elastic, and, therefore, the pressure 𝑝 is found by 𝑝 = −𝐾𝜀𝑣, (22.66.3) where 𝜀𝑣 is the volumetric strain. LS-DYNA Theory Manual Material Models 22.67 Material Models 81 and 82: Plasticity with Damage and Orthotropic Option With this model an elasto-viscoplastic material with an arbitrary stress versus strain curve and arbitrary strain rate dependency can be defined. Damage is considered before rupture occurs. Also, failure based on a plastic strain or a minimum time step size can be defined. An option in the keyword input, ORTHO, is available, which invokes an orthotropic damage model. This option is an extension to include orthotropic damage as a means of treating failure in aluminum panels. Directional damage begins after a defined failure strain is reached in tension and continues to evolve until a tensile rupture strain is reached in either one of the two orthogonal directions. The stress versus strain behavior may be treated by a bilinear stress strain curve by defining the tangent modulus, ETAN. Alternately, a curve similar to that shown in Figure 22.67.1 is expected to be defined by (EPS1,ES1) - (EPS8,ES8); however, an effective stress versus effective plastic strain curve (LCSS) may be input instead if eight points are insufficient. The cost is roughly the same for either approach. The most yield yield stress versus effective plastic strain for undamaged material Failure Begins damage increases linearly with plastic strain after failure nominal stress after failure rupture ω=0 ω=1 εp eff Figure .22.67.1. Stress strain behavior when damage is included. general approach is to use the table definition (LCSS) discussed below. Two options to account for strain rate effects are possible. Strain rate may be accounted for using the Cowper-Symonds model which scales the yield stress with the factor, Material Models LS-DYNA Theory Manual 1 + ( 𝑝⁄ ) , 𝜀̇ (22.67.1) where 𝜀̇ is the strain rate, 𝜀̇ = √𝜀̇𝑖𝑗𝜀̇𝑖𝑗. If the viscoplastic option is active, VP = 1.0, and if SIGY is > 0 then the dynamic yield stress is computed from the sum of the static stress, p ), which is typically given by a load curve ID, and the initial yield stress, SIGY, s(𝜀eff 𝜎y multiplied by the Cowper-Symonds rate term as follows: 𝜎𝑦(𝜀eff p , 𝜀̇eff p ) = 𝜎𝑦 s(𝜀eff p ) + SIGY ⋅ ( p⁄ ) , 𝜀̇eff (22.67.2) where the plastic strain rate is used. With this latter approach similar results can be obtained model: model *MAT_ANISOTROPIC_VISCOPLASTIC. If SIGY = 0, the following equation is used instead where the static stress, 𝜎y p ), must be defined by a load curve: between material and this s(𝜀eff 𝜎y(𝜀eff p , 𝜀̇eff p ) = 𝜎y p ) s(𝜀eff 𝜀̇eff ) ⎡ 1 + ( ⎢⎢ ⎣ p⁄ ⎤ . ⎥⎥ ⎦ (22.67.3) This latter equation is always used if the viscoplastic option is off. For complete generality a load curve (LCSR) to scale the yield stress may be input instead. In this curve the scale factor versus strain rate is defined. The constitutive properties for the damaged material are obtained from the undamaged material properties. The amount of damage evolved is represented by the constant, 𝜔, which varies from zero if no damage has occurred to unity for complete rupture. For uniaxial loading, the nominal stress in the damaged material is given by where P is the applied load and A is the surface area. The true stress is given by: 𝜎nominal = , (22.67.4) 𝜎true = 𝐴 − 𝐴loss , where 𝐴loss is the void area. The damage variable can then be defined: 𝜔 = 𝐴loss , 0 ≤ 𝜔 ≤ 1. (22.67.5) (22.67.6) In this model damage is defined in terms of plastic strain after the failure strain is exceeded: 𝜔 = p − 𝜀failure 𝜀eff − 𝜀failure 𝜀rupture if 𝜀failure ≤ 𝜀eff p ≤ 𝜀rupture . (22.67.7) LS-DYNA Theory Manual Material Models After exceeding the failure strain softening begins and continues until the rupture strain is reached. By default, deletion of a shell element occurs when all integration points in the shell have failed. A parameter is available, NUMINT, that defines the number of through thickness integration points for shell element deletion. The default of all integration points is not recommended since shells undergoing large strain are often not deleted due to nodal fiber rotations which limit strains at active integration points after most points have failed. Better results are obtained if NUMINT is set to 1 or a number less than one half of the number of through thickness points. For example, if four through thickness points are used, NUMINT should not exceed 2, even for fully integrated shells which have 16 integration points. 22.67.1 Material Model 82: Isotropic Elastic-Plastic with Anisotropic Damage Material 82 is an isotropic elastic-plastic material model with anisotropic damage.. The stress update in the case of shell elements is performed as follows. For a 𝑡, 𝑖 = 1, 2 at time 𝑡, the local stress is given stress state 𝜎𝑖𝑗 obtained as 𝑡 and damage parameters 𝐷𝑖 𝑡 , 𝑙 = 𝑞𝑘𝑖𝑞𝑙𝑗𝜎𝑘𝑙 𝜎𝑖𝑗 (22.67.8) where 𝑞𝑖𝑗 is an orthogonal matrix determining the direction of the damage. The directions are determined as follows. The first direction is taken as the one in which the plastic strain first reaches the plastic strain at impending failure, see below. The other direction is orthogonal to the first and in the plane of the shell. ε eff p - f s failure Figure 22.67.2. A nonlinear damage curve is optional. Note that the origin of the curve is at (0,0). It is permissible to input the failure strain, fs, as zero for this option. The nonlinear damage curve is useful for controlling the softening behavior after the failure strain is reached. For this local stress, the undamaged stress is computed as Material Models LS-DYNA Theory Manual u = 𝜎11 u = 𝜎22 u = 𝜎12 u = 𝜎23 u = 𝜎13 t , 𝜎11 1 − D1 𝜎22 𝑡 , 1 − D2 2𝜎12 𝑡 , 2 − 𝐷1 𝜎23 1 − 𝐷2 𝜎13 𝑡 . 1 − 𝐷1 𝑡 , 𝑡 − 𝐷2 (22.67.9) A new undamaged stress 𝜎𝑖𝑗 u+ is then computed following a standard elastic- plastic stress update. The damage at the next time step is computed according to p − 𝜀f 𝜀𝑖𝑖 𝜀r − 𝜀f 𝑡+ = max (𝐷𝑖 𝑡, 𝑖 = 1, 2, 𝐷𝑖 ) , (22.67.10) where 𝜀f is the plastic strain at impending failure, 𝜀r is the plastic strain at rupture and p is the current plastic strain in the local 𝑖 direction. There is also an option of defining 𝜀𝑖𝑖 a nonlinear damage curve, with this option the new damage is computed as 𝑡, 𝑓 (𝜀𝑖𝑖 𝑡+ = max(𝐷𝑖 p − 𝜀f)), 𝑖 = 1, 2, (22.67.11) 𝐷𝑖 for a user-defined load curve 𝑓 . The new local (damaged) stress is given by l+ = 𝜎11 𝜎11 l+ = 𝜎22 𝜎22 l+ = 𝜎12 𝜎12 l+ = 𝜎23 𝜎23 l+ = 𝜎13 𝜎13 𝑡+), u+(1 − 𝐷1 𝑡+), u+(1 − 𝐷2 t+ t+ − 𝐷2 u+ 2 − 𝐷1 t+), u+(1 − 𝐷2 t+), u+(1 − 𝐷1 , (22.67.12) which is transformed back to the local system to obtain the new global damaged stress as 𝑙+. 𝑡+ = 𝑞𝑖𝑘𝑞𝑗𝑙𝜎𝑘𝑙 𝜎𝑖𝑗 (22.67.13) An integration point is completely failed, i.e., it is removed from the calculations, when max(𝐷1, 𝐷2) > 0.999. The element is removed from the model when a user specified number of integration points in that element have failed. LS-DYNA Theory Manual Material Models There are options of using visco-plasticity in the current model. The details of this part of the stress update is omitted here. The Rc-Dc Damage Model The Rc-Dc model is defined as the following, see the report on the Fundamental Study of Crack Initiation and Propagation [2003]. The damage 𝐷 is updated as 𝐷𝑡+ = 𝐷𝑡 + 𝜔1𝜔2Δ𝜀p (22.67.14) where Δ𝜀p is the plastic strain increment and 𝜔1 = (1 + 𝛾𝑝)−𝛼, 𝜔2 = (2 − 𝐴𝐷)𝛽. (22.67.15) Here 𝑝 is the pressure, 𝛼, 𝛽 and 𝛾 are material parameters and 𝐴𝐷 = ⎧ {{ ⎨ {{ ⎩ 1.9999 if max(𝑆1, 𝑆2) ≤ 0 min (∣ 𝑆1 𝑆2 ∣ , ∣ 𝑆2 𝑆1 ∣) otherwise . (22.67.16) where 𝑆1 and 𝑆2 are the in-plane principal stress values. Fracture is initiated when the accumulation of damage is greater than a critical damage 𝐷c given by 𝐷c = 𝐷0(1 + 𝑏‖∇𝐷‖𝜆). (22.67.17) Here 𝐷0, 𝑏 and λ are material parameters and ∇D is the spatial gradient of damage. We have added an option to use a non-local formulation with 𝐷 as the non-local variable and a characteristic length 𝑙. More information on this can be found in the LS-DYNA Keyword User’s Manual [Hallquist 2003]. With this option we compute 𝐷c as, 𝐷c = 𝐷0, (22.67.18) hence the parameters 𝑏 and 𝜆 are not used. A fracture fraction given by 𝐹 = 𝐷 − 𝐷c 𝐷s (22.67.19) defines the degradations of the material by the Rc-Dc model. Here 𝐷s is yet another parameter determined by the user. The stress update of material 82 is modified accordingly. Upon entry the stress is divided by the factor 1 − 𝐹𝑡 to account for the Rc-Dc damage. Before exiting the routine, the stress is multiplied by the new Rc-Fc (reversed) fracture fraction 1 − 𝐹𝑡+. An integration point is considered failed when min(1 − 𝐷1, 1 − 𝐷2)(1 − 𝐹) < 0.001. Material Models LS-DYNA Theory Manual 22.68 Material Model 83: Fu-Chang’s Foam With Rate Effects This model allows rate effects to be modeled in low and medium density foams, see Figure 22.68.1. Hysteretic unloading behavior in this model is a function of the rate sensitivity with the most rate sensitive foams providing the largest hysteresis and visa versa. The unified constitutive equations for foam materials by Fu-Chang [1995] provide the basis for this model. This implementation incorporates the coding in the reference in modified form to ensure reasonable computational efficiency. The mathematical description given below is excerpted from the reference. The strain is divided into two parts: a linear part and a non-linear part of the strain and the strain rate becomes 𝐄(𝑡) = 𝐄L(𝑡) + 𝐄N(𝑡), 𝐄̇(𝑡) = 𝐄̇L(𝑡) + 𝐄̇N(𝑡). (22.68.1) (22.68.2) 𝐄̇N is an expression for the past history of 𝐄N. A postulated constitutive equation may be written as: Figure 22.68.1. Rate effects in Fu Chang’s foam model. 1-V LS-DYNA Theory Manual Material Models ∞ 𝛔(𝑡) = ∫ [𝐄𝑡 N(𝜏), 𝐒(𝑡)] 𝑑𝜏, 𝜏=0 (22.68.3) where 𝐒(𝑡) is the state variable and ∫ ∞ and ∞ 𝜏=0 is a functional of all values of 𝜏 in 𝑇𝜏: 0 ≤ 𝜏 ≤ where 𝜏 is the history parameter: N(𝜏) = 𝐄N(𝑡 − 𝜏), 𝐄𝑡 N(𝜏 = ∞) ⇔ the virgin material. 𝐄𝑡 (22.68.4) (22.68.5) It is assumed that the material remembers only its immediate past, i.e., a N(𝜏) in a Taylor series about neighborhood about 𝜏 = 0. Therefore, an expansion of 𝐄𝑡 𝜏 = 0 yields: N(𝜏) = 𝐄N(0) + 𝐄𝑡 𝜕𝐄𝑡 𝜕𝑡 (0)𝑑𝑡. Hence, the postulated constitutive equation becomes: 𝛔(𝑡) = 𝛔∗(𝐄N(𝑡), 𝐄̇N(𝑡), 𝐒(𝑡)), where we have replaced ∂𝐄𝑡 ∂𝑡 by 𝐄̇N, and 𝛔∗ is a function of its arguments. For a special case, we may write 𝛔(𝑡) = 𝛔∗(𝐄̇N(𝑡), 𝐒(𝑡)), N = 𝑓 (𝐒(𝑡), 𝐬(𝑡)), 𝐄̇𝑡 (22.68.6) (22.68.7) (22.68.8) (22.68.9) which states that the nonlinear strain rate is the function of stress and a state variable which represents the history of loading. Therefore, the proposed kinetic equation for foam materials is: 𝐄̇N = ‖𝛔‖ 𝐷0exp [−𝑐0 ( 2𝑛0 tr(𝛔𝐒) (‖𝛔‖)2 ) ], (22.68.10) where 𝐷0, 𝑐0, and 𝑛0 are material constants, and 𝐒 is the overall state variable. If either 𝐷0 = 0 or 𝑐0 → ∞ then the nonlinear strain rate vanishes. 𝑆̇𝑖𝑗 = [𝑐1(𝑎𝑖𝑗𝑅 − 𝑐2𝑆𝑖𝑗)𝑃 + 𝑐3𝑊𝑛1(∥𝐸̇𝑁∥) 𝑛2𝐼𝑖𝑗]𝑅 𝑅 = 1 + 𝑐4 𝑛3 ∥𝐄̇N∥ 𝑐5 ⎜⎛ ⎝ − 1 ⎟⎞ ⎠ 𝑃 = tr(𝛔𝐄̇N) (22.68.11) (22.68.12) (22.68.13) Material Models LS-DYNA Theory Manual where 𝑐1, 𝑐2, 𝑐3, 𝑐4, 𝑐5, 𝑛1, 𝑛2, 𝑛3, and 𝑎𝑖𝑗 are material constants and: W = ∫ tr(𝛔𝑑𝐄), (22.68.14) 2, ‖𝛔‖ = (𝜎𝑖𝑗𝜎𝑖𝑗) ∥𝐄̇∥ = (𝐸̇𝑖𝑗𝐸̇𝑖𝑗) 2, N) 2. ∥𝐄̇N∥ = (𝐸̇𝑖𝑗 N𝐸̇𝑖𝑗 (22.68.15) In the implementation by Fu Chang the model was simplified such that the input constants 𝑎𝑖𝑗 and the state variables 𝑆𝑖𝑗 are scalars. Viscous damping in the model follows an implementation identical to that of material type 57. LS-DYNA Theory Manual Material Models 22.69 Material Model 84 and 85: Winfrith Concrete Pressure is positive in compression; volumetric strain is given by the natural log of the relative volume and is negative in compression. The tabulated data are given in order of increasing compression, with no initial zero point. If the volume compaction curve is omitted, the following scaled curve is automatically used where 𝑝1 is the pressure at uniaxial compressive failure computed from: 𝑝1 = 𝜎𝑐 , and 𝐾 is the unloading bulk modulus computed from 𝐾 = 𝐸s , 3(1 − 2𝑣) where 𝐸s is the input tangent modulus for concrete and 𝑣 is Poisson's ratio. (22.69.1) (22.69.2) Volumetric Strain −𝑝1/K -0.002 -0.004 -0.010 -0.020 -0.030 -0.041 -0.051 -0.062 -0.094 Pressure (MPa) 1.00 × 𝑝1 1.50 × 𝑝1 3.00 × 𝑝1 4.80 × 𝑝1 6.00 × 𝑝1 7.50 × 𝑝1 9.45 × 𝑝1 11.55 × 𝑝1 14.25 × 𝑝1 25.05 × 𝑝1 Table 22.3. Default pressure versus volumetric strain curve for concrete if the curve is not defined. Material Models LS-DYNA Theory Manual 22.70 Material Model 87: Cellular Rubber This material model provides a cellular rubber model combined with linear viscoelasticity as outlined by Christensen [1980]. Rubber is generally considered to be fully incompressible since the bulk modulus greatly exceeds the shear modulus in magnitude. To model the rubber as an unconstrained material a hydrostatic work term, 𝑊𝐻(𝐽), is included in the strain energy functional which is function of the relative volume, 𝐽, [Ogden, 1984]: 𝑊(𝐽1, 𝐽2, 𝐽) = ∑ 𝐶𝑝𝑞 (𝐽1 − 3)𝑝(𝐽2 − 3)𝑞 + 𝑊𝐻(𝐽) 𝑝,𝑞=0 −1 3⁄ 𝐽1 = 𝐼1𝐼3 𝐽2 = 𝐼2𝐼3 −2 3⁄ (22.70.1) In order to prevent volumetric work from contributing to the hydrostatic work the first and second invariants are modified as shown. This procedure is described in more detail by Sussman and Bathe [1987]. The effects of confined air pressure in its overall response characteristics are included by augmenting the stress state within the element by the air pressure. 𝜎𝑖𝑗 = 𝜎𝑖𝑗 sk − 𝛿𝑖𝑗𝜎 air, (22.70.2) sk is the bulk skeletal stress and σair is the air pressure computed from the where 𝜎𝑖𝑗 equation: 𝜎 air = − 𝑝0𝛾 1 + 𝛾 − 𝜙 , (22.70.3) where 𝑝0 is the initial foam pressure usually taken as the atmospheric pressure and 𝛾 defines the volumetric strain where 𝑉 is the relative volume of the voids and 𝛾0 is the initial volumetric strain which is typically zero. The rubber skeletal material is assumed to be incompressible. 𝛾 = 𝑉 − 1 + 𝛾0, (22.70.4) Rate effects are taken into account through linear viscoelasticity by a convolution integral of the form: 𝜎𝑖𝑗 = ∫ 𝑔𝑖𝑗𝑘𝑙 (𝑡 − 𝜏) 𝜕𝜀𝑘𝑙 𝜕𝜏 𝑑𝜏, (22.70.5) or in terms of the second Piola-Kirchhoff stress, 𝑆𝑖𝑗, and Green's strain tensor, 𝐸𝑖𝑗, LS-DYNA Theory Manual Material Models 𝑆𝑖𝑗 = ∫ 𝐺𝑖𝑗𝑘𝑙 (𝑡 − 𝜏) 𝜕𝐸𝑘𝑙 𝜕𝜏 𝑑𝜏, (22.70.6) where 𝑔𝑖𝑗𝑘𝑙(𝑡 − 𝜏) and 𝐺𝑖𝑗𝑘𝑙(𝑡 − 𝜏) are the relaxation functions for the different stress measures. This stress is added to the stress tensor determined from the strain energy functional. Since we wish to include only simple rate effects, the relaxation function is represented by one term from the Prony series: given by, 𝑔(𝑡) = 𝛼0 + ∑ 𝛼𝑚 𝑚=1 𝑒−𝛽𝑡, 𝑔(𝑡) = 𝐸𝑑𝑒−𝛽1𝑡. (22.70.7) (22.70.8) This model is effectively a Maxwell fluid which consists of a damper and spring in series. We characterize this in the input by a shear modulus, 𝐺, and decay constant, 𝛽1. The Mooney-Rivlin rubber model is obtained by specifying 𝑛 = 1. In spite of the differences in formulations with Model 27, we find that the results obtained with this model are nearly identical with those of 27 as long as large values of Poisson’s ratio are used. Rubber Block with Entrapped Air Air Figure 22.70.1. Cellular rubber with entrapped air. By setting the initial air pressure to zero, an open cell, cellular rubber can be simulated. Material Models LS-DYNA Theory Manual 22.71 Material Model 88: MTS Model The Mechanical Threshhold Stress (MTS) model is due to Mauldin, Davidson, and Henninger [1990] and is available for applications involving large strains, high pressures and strain rates. As described in the foregoing reference, this model is based on dislocation mechanics and provides a better understanding of the plastic deformation process for ductile materials by using an internal state variable called the mechanical threshold stress. This kinematic quantity tracks the evolution of the material’s microstructure along some arbitrary strain, strain rate, and temperature- dependent path using a differential form that balances dislocation generation and recovery processes. Given a value for the mechanical threshold stress, the flow stress is determined using either a thermal-activation-controlled or a drag-controlled kinetics relationship. An equation-of-state is required for solid elements and a bulk modulus must be defined below for shell elements. The flow stress 𝜎 is given by: 𝜎 = 𝜎̂a + 𝐺0 [𝑠th𝜎̂ + 𝑠th,𝑖𝜎̂𝑖 + 𝑠th,𝑠𝜎̂s]. (22.71.1) The first product in the equation for 𝜎 contains a micro-structure evolution variable, i.e., 𝜎̂ , called the Mechanical Threshold Stress (MTS), that is multiplied by a constant- structure deformation variable 𝑠th:𝑠th is a function of absolute temperature 𝑇 and the plastic strain-rates 𝜀̇P. The evolution equation for 𝜎̂ is a differential hardening law representing dislocation-dislocation interactions: ∂σ̂ ∂𝜀p ≡ Θo 1 − ⎡ ⎢ ⎢ ⎢ ⎣ tanh (α σ̂ 𝜎̂εs tanh(𝛼) ) . ⎤ ⎥ ⎥ ⎥ ⎦ (22.71.2) The term, ∂𝜎̂ ∂𝜀p, represents the hardening due to dislocation generation and the stress ratio, 𝜎̂ , represents softening due to dislocation recovery. The threshold stress at 𝜎̂εs zero strain-hardening 𝜎̂εs is called the saturation threshold stress. Relationships for 𝛩𝑜, 𝜎̂εs are: 𝛩𝑜 = 𝑎𝑜 + 𝑎1ln ( 𝜀̇p 𝜀0 ) + 𝑎2√ 𝜀̇p 𝜀0 , (22.71.3) which contains the material constants 𝑎o, 𝑎1, and 𝑎2. The constant, 𝜎̂εs, is given as: 𝜎̂εs = 𝜎̂εso ( 𝑘𝑇/𝐺𝑏3𝐴 , 𝜀̇𝑝 𝜀̇εso ) (22.71.4) LS-DYNA Theory Manual Material Models which contains the input constants: 𝜎̂εso, 𝜀̇εso, 𝑏, 𝐴, and 𝑘. The shear modulus 𝐺 appearing in these equations is assumed to be a function of temperature and is given by the correlation. 𝐺 = 𝐺0 − 𝑏1 , 𝑏2 𝑇 − 1 which contains the constants: 𝐺0, 𝑏1, and 𝑏2. For thermal-activation controlled deformation 𝑠th is evaluated via an Arrhenius rate equation of the form: (22.71.5) ⎜⎜⎜⎜⎜⎛𝑘𝑇ln ( 𝐺𝑏3𝑔0 𝜀̇0 𝜀̇p) ⎟⎟⎟⎟⎟⎞ 𝑠th = 1 − ⎡ ⎢ ⎢ ⎢ ⎢ ⎣ ⎝ ⎤ ⎥ ⎥ ⎥ ⎥ ⎦ . (22.71.6) ⎠ The absolute temperature is given as: where 𝐸 in the internal energy density per unit initial volume. 𝑇 = 𝑇ref + 𝜌𝑐p𝐸, (22.71.7) Material Models LS-DYNA Theory Manual 22.72 Material Model 89: Plasticity Polymer Unlike other LS-DYNA material models, both the input stress-strain curve and the strain to failure are defined as total true strain, not plastic strain. The input can be defined from uniaxial tensile tests; nominal stress and nominal strain from the tests must be converted to true stress and true strain. The elastic component of strain must not be subtracted out. The stress-strain curve is permitted to have sections steeper (i.e. stiffer) than the elastic modulus. When these are encountered the elastic modulus is increased to prevent spurious energy generation. LS-DYNA Theory Manual Material Models 22.73 Material Model 90: Acoustic This model is appropriate for tracking low-pressure stress waves in an acoustic media such as air or water and can be used only with the acoustic pressure element formulation. The acoustic pressure element requires only one unknown per node. This element is very cost effective. Material Models LS-DYNA Theory Manual 22.74 Material Model 91: Soft Tissue The overall strain energy W is "uncoupled" and includes two isotropic deviatoric matrix terms, a fiber term F, and a bulk term: 𝑊 = 𝐶1(𝐼 ̃1 − 3) + 𝐶2(𝐼 ̃2 − 3) + 𝐹(𝜆) + 𝐾[ln(𝐽)]2. (22.74.1) Here, 𝐼 ̃1 and 𝐼 ̃2 are the deviatoric invariants of the right Cauchy deformation tensor, 𝜆 is the deviatoric part of the stretch along the current fiber direction, and 𝐽 = det𝐅 is the volume ratio. The material coefficients 𝐶1 and 𝐶2 are the Mooney-Rivlin coefficients, while 𝐾 is the effective bulk modulus of the material (input parameter XK). The derivatives of the fiber term 𝐹 are defined to capture the behavior of crimped collagen. The fibers are assumed to be unable to resist compressive loading - thus the model is isotropic when 𝜆 < 1. An exponential function describes the straightening of the fibers, while a linear function describes the behavior of the fibers once they are straightened past a critical fiber stretch level 𝜆 ≥ 𝜆∗ (input parameter XLAM): ∂𝐹 ∂λ = ⎧0 {{{ 𝐶3 ⎨ {{{ ⎩ 𝜆 < 1 [exp(𝐶4(𝜆 − 1)) − 1] 𝜆 < 𝜆∗ . (22.74.2) (𝐶5𝜆 + 𝐶6) 𝜆 ≥ 𝜆∗ Coefficients 𝐶3, 𝐶4, and 𝐶5 must be defined by the user. 𝐶6 is determined by LS-DYNA to ensure stress continuity at 𝜆 = 𝜆∗. Sample values for the material coefficients 𝐶1 − 𝐶5 and 𝜆∗ for ligament tissue can be found in Quapp and Weiss [1998]. The bulk modulus K should be at least 3 orders of magnitude larger than 𝐶1 to ensure near-incompressible material behavior. Viscoelasticity is included via a convolution integral representation for the time- dependent second Piola-Kirchoff stress 𝐒(𝐂, 𝑡): 𝐒(𝐂, 𝑡) = 𝐒e(𝐂) + ∫ 2𝐺(𝑡 − 𝑠) ∂W ∂𝐂(s) 𝑑𝑠. (22.74.3) Here, 𝐒e is the elastic part of the second PK stress as derived from the strain energy, and 𝐺(𝑡 − 𝑠) is the reduced relaxation function, represented by a Prony series: 𝐺(t) = ∑ S𝑖 𝑖=1 exp ( 𝑇𝑖 ). (22.74.4) Puso and Weiss [1998] describe a graphical method to fit the Prony series coefficients to relaxation data that approximates the behavior of the continuous relaxation function proposed by Y-C. Fung, as quasilinear viscoelasticity. LS-DYNA Theory Manual Material Models 22.75 Material Model 94: Inelastic Spring Discrete Beam The yield force is taken from the load curve: 𝐹Y = 𝐹y(Δ𝐿plastic), where 𝐿plastic is the plastic deflection. A trial force is computed as: and is checked against the yield force to determine F: 𝐹T = 𝐹n + 𝐾 ⋅ Δ𝐿̇ ⋅ Δ𝑡, 𝐹 = {𝐹Y if 𝐹T > 𝐹Y 𝐹T if 𝐹T ≤ 𝐹Y. (22.75.1) (22.75.2) (22.75.3) The final force, which includes rate effects and damping, is given by: 𝐹𝑛+1 = 𝐹 ⋅ [1 + 𝐶1 ⋅ Δ𝐿̇ + 𝐶2 ⋅ sgn(Δ𝐿̇)ln (max {1. , ∣Δ𝐿̇∣ DLE })] + DΔ𝐿̇ + 𝑔(𝛥𝐿)ℎ(𝛥𝐿̇), (22.75.4) where 𝐶1, 𝐶2 are damping coefficients, DLE is a factor to scale time units. Unless the origin of the curve starts at (0,0), the negative part of the curve is used when the spring force is negative where the negative of the plastic displacement is used to interpolate, 𝐹y. The positive part of the curve is used whenever the force is positive. In these equations, Δ𝐿 is the change in length Δ𝐿 = current length-initial length. (22.75.5) Material Models LS-DYNA Theory Manual 22.76 Material Model 96: Brittle Damage Model A full description of the tensile and shear damage parts of this material model is given in Govindjee, Kay and Simo [1994,1995]. It is an anisotropic brittle damage model designed primarily for concrete, though it can be applied to a wide variety of brittle materials. It admits progressive degradation of tensile and shear strengths across smeared cracks that are initiated under tensile loadings. Compressive failure is governed by a simplistic J2 flow correction that can be disabled if not desired. Damage is handled by treating the rank 4 elastic stiffness tensor as an evolving internal variable for the material. Softening induced mesh dependencies are handled by a characteristic length method [Oliver 1989]. Description of properties: 1. 2. 3. 𝐸 is the Young's modulus of the undamaged material also known as the virgin modulus. 𝜐 is the Poisson's ratio of the undamaged material also known as the virgin Poisson's ratio. 𝑓𝑛 is the initial principal tensile strength (stress) of the material. Once this stress has been reached at a point in the body a smeared crack is initiated there with a normal that is co-linear with the 1st principal direction. Once initiated, the crack is fixed at that location, though it will convect with the motion of the body. As the loading progresses the allowed tensile traction normal to the crack plane is progressively degraded to a small machine dependent constant. The degradation is implemented by reducing the material's modulus normal to the smeared crack plane according to a maximum dissipation law that incorpo- rates exponential softening. The restriction on the normal tractions is given by 𝜙t = (𝐧 ⊗ 𝐧): 𝛔 − 𝑓n + (1 − 𝜀)𝑓n(1 − exp[−𝐻𝛼]) ≤ 0, (22.76.1) where 𝐧 is the smeared crack normal, 𝜀 is the small constant, 𝐻 is the softening modulus, and 𝛼 is an internal variable. 𝐻 is set automatically by the program; see 𝑔c below. 𝛼 measures the crack field intensity and is output in the equiva- lent plastic strain field, 𝜀̅p, in a normalized fashion. The evolution of alpha is governed by a maximum dissipation argument. When the normalized value reaches unity it means that the material's strength has been reduced to 2% of its original value in the normal and parallel direc- tions to the smeared crack. Note that for plotting purposes, it is never output greater than 5. LS-DYNA Theory Manual Material Models 4. 5. 6. 7. 8. 𝑓s is the initial shear traction that may be transmitted across a smeared crack plane. The shear traction is limited to be less than or equal to 𝑓s(1 − 𝛽)(1 − exp[−𝐻𝛼]), through the use of two orthogonal shear damage surfaces. Note that the shear degradation is coupled to the tensile degradation through the internal variable alpha which measures the intensity of the crack field. 𝛽 is the shear retention factor defined below. The shear degradation is taken care of by reducing the material's shear stiffness parallel to the smeared crack plane. 𝑔c is the fracture toughness of the material. It should be entered as fracture energy per unit area crack advance. Once entered the softening modulus is automatically calculated based on element and crack geometries. 𝛽 is the shear retention factor. As the damage progresses the shear tractions allowed across the smeared crack plane asymptote to the product 𝛽𝑓s. 𝜂 represents the viscosity of the material. Viscous behavior is implemented as a simple Perzyna regularization method. This allows for the inclusion of first order rate effects. The use of some viscosity is recommend as it serves as regu- larizing parameter that increases the stability of calculations. 𝜎y is a uniaxial compressive yield stress. A check on compressive stresses is made using the J2 yield function s: s − √2 3 𝜎y ≤ 0, where s is the stress deviator. If violated, a J2 return mapping correction is executed. This check is executed when (1) no damage has taken place at an integration point yet, (2) when damage has taken place at a point but the crack is currently closed, and (3) during active damage after the damage integration (ie. as an operator split). Note that if the crack is open, the plasticity correction is done in the plane- stress subspace of the crack plane. Remark: A variety of experimental data has been replicated using this model from quasi-static to explosive situations. Reasonable properties for a standard grade concrete would be 𝐸 = 3.15 × 106psi, 𝑓n = 450 psi, 𝑓s = 2100 psi, 𝑣 = 0.2, 𝑔c = 0.8 lbs/in, 𝛽 = 0.03, 𝜂 = 0.0 psi-sec, 𝜎y = 4200 psi. For stability, values of 𝜂 between 104 to 106 psi/sec are recommended. Our limited experience thus far has shown that many problems require nonzero values of 𝜂 to run to avoid error terminations. Various other internal variables such as crack orientations and degraded stiffness tensors are internally calculated but currently not available for output. Material Models LS-DYNA Theory Manual 22.77 Material Model 97: General Joint Discrete Beam For explicit calculations, the additional stiffness due to this joint may require additional mass and inertia for stability. Mass and rotary inertia for this beam element is based on the defined mass density, the volume, and the mass moment of inertia defined in the *SECTION_ BEAM input. The penalty stiffness applies to explicit calculations. For implicit calculations, constraint equations are generated and imposed on the system equations; therefore, these constants, RPST and RPSR, are not used. LS-DYNA Theory Manual Material Models 22.78 Material Model 98: Simplified Johnson Cook Johnson and Cook express the flow stress as 𝜎𝑦 = (𝐴 + 𝐵𝜀̅ p𝑛 ) (1 + 𝐶ln𝜀̇∗), (22.78.1) where 𝐴, 𝐵, 𝐶 and 𝑛 are input constants 𝜀̅p effective plastic strain 𝜀̇∗ = 𝜀̅ 𝜀̇0 effective strain rate for 𝜀̇0 = 1s−1 The maximum stress is limited by SIGMAX and SIGSAT by: 𝜎y = min {min [𝐴 + 𝐵𝜀̅ p𝑛 , SIGMAX] (1 + 𝐶ln𝜀̇∗), SIGSAT}. (22.78.2) Failure occurs when the effective plastic strain exceeds PSFAIL. If the viscoplastic option is active, VP = 1.0, the parameters SIGMAX and SIGSAT are ignored since these parameters make convergence of the viscoplastic strain iteration loop difficult to achieve. The viscoplastic option replaces the plastic strain in the forgoing equations by the viscoplastic strain and the strain rate by the viscoplastic strain rate. Numerical noise is substantially reduced by the viscoplastic formulation. LS-DYNA Draft Material Models LS-DYNA Theory Manual 22.79 Material Model 100: Spot Weld This material model applies to beam element type 9 for spot welds. These beam elements may be placed between any two deformable shell surfaces, see Figure 22.79.1, and tied with type 7 constraint contact which eliminates the need to have adjacent nodes at spot weld locations. Beam spot welds may be placed between rigid bodies and rigid/deformable bodies by making the node on one end of the spot weld a rigid body node which can be an extra node for the rigid body. In the same way, rigid bodies may also be tied together with this spot weld option. It is advisable to include all spot welds, which provide the slave nodes, and spot welded materials, which define the master segments, within a single type 7 tied interface. As a constraint method, multiple type 7 interfaces are treated independently which can lead to significant problems if such interfaces share common nodal points. The offset option, “o 7”, should not be used with spot welds. The DAMAGE-FAILURE option causes one additional line to be read with the damage parameter and a flag that determines how failure is computed from the resultants. On this line the parameter, DMG, if nonzero, invokes damage mechanics combined with the plasticity model to achieve a smooth drop off of the resultant forces prior to the removal of the spot weld. The parameter FOPT determines the method used in computing resultant based failure, which is unrelated to damage. The weld material is modeled with isotropic hardening plasticity coupled to two failure models. The first model specifies a failure strain which fails each integration SPOTWELD ELEMENT Trr Frr Mtt Mss Frt Frs n2 n1 Figure 22.79.1. Deformable spotwelds can be arbitrarily placed within the structure. LS-DYNA Theory Manual Material Models point in the spot weld independently. The second model fails the entire weld if the resultants are outside of the failure surface defined by: ( 𝑁𝑟𝑟 𝑁𝑟𝑟F ) + ( 𝑁𝑟𝑠 𝑁𝑟𝑠F ) + ( 𝑁𝑟𝑡 𝑁𝑟𝑡F ) + ( 𝑀𝑟𝑟 𝑀𝑟𝑟F ) + ( 𝑀𝑠𝑠 𝑀𝑠𝑠F ) + ( 𝑇𝑟𝑟 𝑇𝑟𝑟F ) − 1 = 0, (22.79.1) where the numerators in the equation are the resultants calculated in the local coordinates of the cross section, and the denominators are the values specified in the input. If the user defined parameter, NF, which the number of force vectors stored for filtering, is nonzero the resultants are filtered before failure is checked. The default value is set to zero which is generally recommended unless oscillatory resultant forces are observed in the time history databases. Even though these welds should not oscillate significantly, this option was added for consistency with the other spot weld options. NF affects the storage since it is necessary to store the resultant forces as history variables. If the failure strain is set to zero, the failure strain model is not used. In a similar manner, when the value of a resultant at failure is set to zero, the corresponding term in the failure surface is ignored. For example, if only N𝑟𝑟F is nonzero, the failure surface is reduced to |N𝑟𝑟| = N𝑟𝑟F. None, either, or both of the failure models may be active depending on the specified input values. The inertias of the spot welds are scaled during the first time step so that their stable time step size is Δ𝑡. A strong compressive load on the spot weld at a later time may reduce the length of the spot weld so that stable time step size drops below Δ𝑡. If the value of Δ𝑡 is zero, mass scaling is not performed, and the spot welds will probably limit the time step size. Under most circumstances, the inertias of the spot welds are small enough that scaling them will have a negligible effect on the structural response and the use of this option is encouraged. Spotweld force history data is written into the SWFORC ASCII file. In this database the resultant moments are not available, but they are in the binary time history database. The constitutive properties for the damaged material are obtained from the undamaged material properties. The amount of damage evolved is represented by the constant, ω, which varies from zero if no damage has occurred to unity for complete rupture. For uniaxial loading, the nominal stress in the damaged material is given by where 𝑃 is the applied load and 𝐴 is the surface area. The true stress is given by: 𝜎nominal = , (22.79.2) 𝜎true = 𝐴 − 𝐴loss , (22.79.3) where 𝐴loss is the void area. The damage variable can then be defined: Material Models LS-DYNA Theory Manual 𝜔 = 𝐴loss , 0 ≤ 𝜔 ≤ 1. (22.79.4) In this model damage is defined in terms of plastic strain after the failure strain is exceeded: 𝜔 = p − 𝜀failure 𝜀eff − 𝜀failure 𝜀rupture if 𝜀failure ≤ 𝜀eff p ≤ 𝜀rupture . (22.79.5) After exceeding the failure strain softening begins and continues until the rupture strain is reached. LS-DYNA Theory Manual Material Models 22.80 Material Model 101: GE Thermoplastics The constitutive model for this approach is: 𝜀̇p = 𝜀̇0exp(𝐴{𝜎 − 𝑆(𝜀p)}) × exp(−𝑝𝛼𝐴), (22.80.1) where 𝜀̇0 and A are rate dependent yield stress parameters, 𝑆(𝜀𝑝) internal resistance (strain hardening) and 𝛼 is a pressure dependence parameter. In this material the yield stress may vary throughout the finite element model as a function of strain rate and hydrostatic stress. Post yield stress behavior is captured in material softening and hardening values. Finally, ductile or brittle failure measured by plastic strain or maximum principal stress respectively is accounted for by automatic element deletion. Although this may be applied to a variety of engineering thermoplastics, GE Plastics have constants available for use in a wide range of commercially available grades of their engineering thermoplastics. Material Models LS-DYNA Theory Manual 22.81 Material Model 102: Hyperbolic Sine Resistance to deformation is both temperature and strain rate dependent. The flow stress equation is: 𝜎 = sinh−1 [ ] ⎜⎜⎛ ⎝ , ⎟⎟⎞ ⎠ where 𝑍, the Zener-Holloman temperature compensated strain rate, is: 𝑍 = 𝜀̇exp ( 𝐺𝑇 ). (22.81.1) (22.81.2) The units of the material constitutive constants are as follows: 𝐴 (1/sec), N (dimensionless), 𝛼 (1/MPa), the activation energy for flow, 𝑄 (J/mol), and the universal gas constant, 𝐺 [J/(mol ⋅ K)]. The value of 𝐺 will only vary with the unit system chosen. Typically it will be either 8.3145 J/(mol ⋅ K), or 40.8825 lb ⋅ in/mol ⋅ R. The final equation necessary to complete the description of high strain rate deformation herein is one that allows computation of the temperature change during the deformation. In the absence of a coupled thermo-mechanical finite element code we assume adiabatic temperature change and follow the empirical assumption that 90-95% of the plastic work is dissipated as heat. Thus the heat generation coefficient is HC ≈ 0.9 𝜌𝐶𝑣 , (22.81.3) where 𝜌 is the material density and 𝐶𝑣 is the specific heat. LS-DYNA Theory Manual Material Models 22.82 Material Model 103: Anisotropic Viscoplastic (22.82.1) (22.82.2) 𝜎(𝜀eff 𝑝 , 𝜀̇eff The uniaxial stress-strain curve is given on the following form 𝑝 )] 𝑝 ) = 𝜎0 + 𝑄𝑟1[(1 − 𝑒𝑥𝑝(−𝐶𝑟1𝜀eff 𝑝 ))] + 𝑉𝑘𝜀̇eff 𝑝 ))] + 𝑄𝑟2[1 − 𝑒𝑥𝑝(−𝐶𝑟2𝜀eff 𝑝 ))] + 𝑄𝜒2[(1 − 𝑒𝑥𝑝(−𝐶𝜒2𝜀eff + 𝑄𝜒1[(1 − 𝑒𝑥𝑝(−𝐶𝜒1𝜀eff 𝑝 𝑉𝑚, For bricks the following yield criteria is used 𝐹(𝜎22 − 𝜎33)2 + 𝐺(𝜎33 − 𝜎11)2 + 𝐻(𝜎11 − 𝜎22)2 + 2𝐿𝜎23 𝑝 )] 𝑝 , 𝜀̇eff 𝑝 is the effective plastic strain and 𝜀̇eff = [𝜎(𝜀eff , 𝑝 is the effective plastic strain rate. For where 𝜀eff shells the anisotropic behavior is given by 𝑅00, 𝑅45 and 𝑅90. When 𝑉𝑘 = 0 the material will behave elasto-plastically. Default values are given by: 2 + 2𝑀𝜎31 2 + 2𝑁𝜎12 𝐹 = 𝐺 = 𝐻 = 𝐿 = 𝑀 = 𝑁 = , , 𝑅00 = 𝑅45 = 𝑅90 = 1. (22.82.3) (22.82.4) (22.82.5) Strain rate is accounted for using the Cowper-Symonds model which, e.g., model 3, scales the yield stress with the factor: 1 + ( 𝑝⁄ ) . 𝜀̇ (22.82.6) To convert these constants set the viscoelastic constants, 𝑉𝑘 and 𝑉𝑚, to the following values: ) , (22.82.7) 𝑉𝑘 = 𝜎 ( 𝑉𝑚 = . This model properly treats rate effects and should provide superior results to models 3 and 24. Material Models LS-DYNA Theory Manual 22.83 Material Model 104: Continuum Damage Mechanics Model Anisotropic Damage model (FLAG = −1). At each thickness integration points, an anisotorpic damage law acts on the plane stress tensor in the directions of the principal total shell strains, ε1 and 𝜀2, as follows: 𝜎11 = (1 − 𝐷1(𝜀1))𝜎110, 𝜎22 = (1 − 𝐷2(𝜀2))𝜎220, 𝜎12 = (1 − 𝐷1 + 𝐷2 ) 𝜎120. (22.83.1) The transverse plate shear stresses in the principal strain directions are assumed to be damaged as follows: 𝜎13 = (1 − 𝜎23 = (1 − 𝐷1 𝐷2 ) 𝜎130, ) 𝜎230. (22.83.2) In the anisotropic damage formulation, 𝐷1(𝜀1) and 𝐷2(𝜀2) are anisotropic damage functions for the loading directions 1 and 2, respectively. Stresses 𝜎110, 𝜎220, 𝜎120, 𝜎130 and 𝜎230 are stresses in the principal shell strain directions as calculated from the undamaged elastic-plastic material behavior. The strains 𝜀1 and 𝜀2 are the magnitude of the principal strains calculated upon reaching the damage thresholds. Damage can only develop for tensile stresses, and the damage functions 𝐷1(𝜀1) and 𝐷2(𝜀2) are identical to zero for negative strains 𝜀1 and 𝜀2. The principal strain directions are fixed within an integration point as soon as either principal strain exceeds the initial threshold strain in tension. A more detailed description of the damage evolution for this material model is given in the description of material 82. The Continuum Damage Mechanics (CDM) model (FLAG≥0) is based on a CDM model proposed by Lemaitre [1992]. The effective stress 𝜎̃ , which is the stress calculated over the section that effectively resist the forces and reads. 𝜎̃ = 1 − 𝐷 , (22.83.3) where 𝐷 is the damage variable. The evolution equation for the damage variable is defined as LS-DYNA Theory Manual Material Models 𝐷̇ = ⎧ {{ ⎨ {{ ⎩ 𝑆(1 − 𝐷) 𝑟 ̇ for 𝑟 > 𝑟𝐷 and 𝜎1 > 0 otherwise . (22.83.4) where 𝑟𝐷 is the damage threshold, 𝑌 is a positive material constant, 𝑆 is the strain energy release rate, and 𝜎1 is the maximal principal stress. The strain energy density release rate is 𝑌 = 𝐞e: 𝐂: 𝐞e = 2 𝑅𝑣 𝜎vm 2𝐸(1 − 𝐷)2, (22.83.5) where 𝜎vm is the equivalent von Mises stress. The triaxiality function 𝑅𝑣 is defined as 𝑅𝑣 = (1 + 𝜈) + 3(1 − 2𝜈) ( 𝜎H 𝜎vm ) . The uniaxial stress-strain curve is given in the following form 𝜎(𝑟, 𝜀̇eff p ) = 𝜎0 + 𝑄1(1 − exp(−𝐶1𝑟)) + 𝑄2(1 − exp(−𝐶2𝑟)) + 𝑉𝑘𝜀̇eff p 𝑉𝑚, where 𝑟 is the damage accumulated plastic strain, which can be calculated by 𝑟 ̇ = 𝜀̇eff p (1 − 𝐷). For bricks the following yield criteria is used 𝐹(𝜎̃22 − 𝜎̃33)2 + 𝐺(𝜎̃33 − 𝜎̃11)2 + 𝐻(𝜎̃11 − 𝜎̃22)2 + 2𝐿𝜎̃23 2 + 2𝑀𝜎̃31 2 + 2𝑁𝜎̃12 = 𝜎(𝑟, 𝜀̇eff p ), (22.83.6) (22.83.7) (22.83.8) (22.83.9) p is the effective viscoplastic where 𝑟 is the damage effective viscoplastic strain and 𝜀̇eff strain rate. For shells the anisotropic behavior is given by the R-values: 𝑅00, 𝑅45, and 𝑅90. When 𝑉𝑘 = 0 the material will behave as an elastoplastic material without rate effects. Default values for the anisotropic constants are given by: 𝐹 = 𝐺 = 𝐻 = 𝐿 = 𝑀 = 𝑁 = , , 𝑅00 = 𝑅45 = 𝑅90 = 1, (22.83.10) (22.83.11) (22.83.12) so that isotropic behavior is obtained. Strain rate is accounted for using the Cowper-Symonds model which scales the yield stress with the factor: Material Models LS-DYNA Theory Manual p⁄ ) . 1 + ( 𝜀̇ (22.83.13) To convert these constants, set the viscoelastic constants, 𝑉𝑘 and 𝑉𝑚, to the following values: ) , (22.83.14) 𝑉𝑘 = 𝜎 ( 𝑉𝑚 = . LS-DYNA Theory Manual Material Models 22.84 Material Model 106: Elastic Viscoplastic Thermal If LCSS is not given any value the uniaxial stress-strain curve has the form p ) = 𝜎0 + 𝑄𝑟1(1 − exp(−𝐶𝑟1𝜀eff 𝜎(𝜀eff +𝑄χ1(1 − exp(−𝐶χ1𝜀eff p )) + Qχ2(1 − exp(−Cχ2𝜀eff p )). p )) + 𝑄𝑟2(1 − exp(−𝐶𝑟2𝜀eff p )) (22.84.1) Viscous effects are accounted for using the Cowper-Symonds model, which scales the yield stress with the factor: 1 + ( p⁄ ) . 𝜀̇eff (22.84.2) Material Models LS-DYNA Theory Manual 22.85 Material Model 110: Johnson-Holmquist Ceramic Model The Johnson-Holmquist plasticity damage model is useful for modeling ceramics, glass and other brittle materials. A more detailed description can be found in a paper by Johnson and Holmquist [1993]. The equivalent stress for a ceramic-type material is given in terms of the damage parameter 𝐷 by Here, 𝜎 ∗ = 𝜎i ∗ − 𝐷(𝜎i ∗ − 𝜎f ∗). ∗ = 𝑎(𝑝∗ + 𝑡∗)𝑛(1 + 𝑐ln𝜀̇∗), 𝜎i (22.85.1) (22.85.2) represents the intact, undamaged behavior. The superscript, '*', indicates a normalized quantity. The stresses are normalized by the equivalent stress at the Hugoniot elastic limit , the pressures are normalized by the pressure at the Hugoniot elastic limit, and the strain rate by the reference strain rate defined in the input. In this equation 𝑎 is the intact normalized strength parameter, 𝑐 is the strength parameter for strain rate dependence, 𝜀̇∗ is the normalized plastic strain rate, and, 𝑡∗ = 𝑝∗ = PHEL PHEL , , (22.85.3) where 𝑇 is the maximum tensile pressure strength, PHEL is the pressure component at the Hugoniot elastic limit, and p is the pressure. p, 𝐷 = ∑ Δ𝜀p/𝜀f (22.85.4) represents the accumulated damage based upon the increase in plastic strain per computational cycle and the plastic strain to fracture p = 𝑑1(𝑝∗ + 𝑡∗)𝑑2, 𝜀f where 𝑑1 and 𝑑2 are user defined input parameters. The equation: ∗ = 𝑏(𝑝∗)𝑚(1 + 𝑐ln𝜀̇∗) ≤ SFMAX, 𝜎f (22.85.5) (22.85.6) represents the damaged behavior where 𝑏 is an input parameter and SFMAX is the maximum normalized fracture strength. The parameter, 𝑑1, controls the rate at which damage accumulates. If it approaches 0, full damage can occur in one time step, i.e., instantaneously. This rate parameter is also the best parameter to vary if one attempts to reproduce results generated by another finite element program. LS-DYNA Theory Manual Material Models In undamaged material, the hydrostatic pressure is given by 𝑝 = 𝑘1𝜇 + 𝑘2𝜇2 + 𝑘3𝜇3, (22.85.7) where 𝜇 = 𝜌/𝜌0 − 1. When damage starts to occur, there is an increase in pressure. A fraction defined in the input, between 0 and 1, of the elastic energy loss, 𝛽, is converted into hydrostatic potential energy, which results in an increase in pressure. The details of this pressure increase are given in the reference. Given HEL and the shear modulus, 𝑔, 𝜇hel can be found iteratively from HEL = 𝑘1𝜇hel + 𝑘2𝜇hel 2 + 𝑘3𝜇hel 3 + 𝑔 ( 𝜇hel 1 + 𝜇hel ), and, subsequently, for normalization purposes, and PHEL = 𝑘1𝜇hel + 𝑘2𝜇hel 2 + 𝑘3𝜇hel 3 , 𝜎hel = 1.5(HEL − PHEL). These are calculated automatically by LS-DYNA if PHEL is zero on input. (22.85.8) (22.85.9) (22.85.10) Material Models LS-DYNA Theory Manual 22.86 Material Model 111: Johnson-Holmquist Concrete Model This model can be used for concrete subjected to large strains, high strain rates, and high pressures. The equivalent strength is expressed as a function of the pressure, strain rate, and damage. The pressure is expressed as a function of the volumetric strain and includes the effect of permanent crushing. The damage is accumulated as a function of the plastic volumetric strain, equivalent plastic strain and pressure. A more detailed description of this model can be found in the paper by Holmquist, Johnson, and Cook [1993] The normalized equivalent stress is defined as 𝜎 ∗ = ′, 𝑓c (22.86.1) where 𝜎 is the actual equivalent stress, and 𝑓c strength. The yield stress is defined in terms of the input parameters 𝑎, 𝑏, 𝑐, and 𝑛 as: ′ is the quasi-static uniaxial compressive 𝜎 ∗ = [𝑎(1 − 𝐷) + 𝑏𝑝∗𝑛][1 − 𝑐ln(𝜀̇∗)], (22.86.2) ′ is the normalized pressure and 𝜀̇∗ = 𝜀̇/𝜀̇0 is where 𝐷 is the damage parameter, 𝑝∗ = 𝑝/𝑓c the dimensionless strain rate. The model accumulates damage both from equivalent plastic strain and plastic volumetric strain, and is expressed as 𝐷 = ∑ Δ𝜀p + Δ𝜇p 𝐷1(𝑝∗ + 𝑇∗)𝐷2 where Δ𝜀p and Δ𝜇p are the equivalent plastic strain and plastic volumetric strain, 𝐷1 ′ is the normalized maximum tensile and 𝐷2 are material constants and 𝑇∗ = 𝑇/𝑓c hydrostatic pressure where 𝑇 is the maximum tensile hydrostatic pressure. (22.86.3) , The pressure for fully dense material is expressed as: 𝑃 = 𝐾1𝜇̅̅̅̅ + 𝐾2𝜇̅̅̅̅2 + 𝐾3𝜇̅̅̅̅3, (22.86.4) where 𝐾1 , 𝐾2 and 𝐾3 are material constants and the modified volumetric strain is defined as 𝜇̅̅̅̅ = 𝜇 − 𝜇lock 1 + 𝜇lock , (22.86.5) where 𝜇lock is the locking volumetric strain. LS-DYNA Theory Manual Material Models 22.87 Material Model 115: Elastic Creep Model The effective creep strain, 𝜀̅c, given as: 𝜀̅c = 𝐴𝜎̅̅̅̅̅ 𝑛𝑡 ̅𝑚, (22.87.1) where 𝐴, 𝑛, and 𝑚 are constants and 𝑡 ̅ is the effective time. The effective stress, 𝜎̅̅̅̅̅, is defined as: 𝜎̅̅̅̅̅ = √ 𝜎𝑖𝑗𝜎𝑖𝑗. (22.87.2) The creep strain, therefore, is only a function of the deviatoric stresses. The volumetric behavior for this material is assumed to be elastic. By varying the time constant 𝑚 primary creep (𝑚 < 1), secondary creep (𝑚 = 1), and tertiary creep (𝑚 > 1) can be modeled. This model is described by Whirley and Henshall (1992). Material Models LS-DYNA Theory Manual 22.88 Material Model 116: Composite Layup This material is for modeling the elastic responses of composite lay-ups that have an arbitrary number of layers through the shell thickness. A pre-integration is used to compute the extensional, bending, and coupling stiffness for use with the Belytschko- Tsay resultant shell formulation. The angles of the local material axes are specified from layer to layer in the *SECTION_SHELL input. This material model must be used with the user defined integration rule for shells, which allows the elastic constants to change from integration point to integration point. Since the stresses are not computed in the resultant formulation, the stress output to the binary databases for the resultant elements are zero. The This material law is based on standard composite lay-up theory. implementation, [Jones 1975], allows the calculation of the force, 𝐍, and moment, 𝐌, stress resultants from: ⎧𝑁𝑥 ⎫ } { 𝑁𝑦 ⎬ ⎨ } { 𝑁𝑥𝑦⎭ ⎩ = 𝐴11 𝐴12 𝐴16 ⎤ ⎡ 𝐴21 𝐴22 𝐴26 ⎥ ⎢ 𝐴16 𝐴26 𝐴66⎦ ⎣ ⎫ ⎧𝜀𝑥 }} {{ 𝜀𝑦 ⎬ ⎨ }} {{ 0⎭ 𝜀𝑧 ⎩ + 𝐵11 𝐵12 𝐵16 ⎤ 𝐵21 𝐵22 𝐵26 ⎥ 𝐵16 𝐵26 𝐵66⎦ ⎡ ⎢ ⎣ {⎧ 𝜅𝑥 }⎫ 𝜅𝑦 𝜅𝑥𝑦⎭}⎬ ⎩{⎨ , ⎧𝑀𝑥 ⎫ } { 𝑀𝑦 ⎬ ⎨ } { 𝑀𝑥𝑦⎭ ⎩ = 𝐵11 𝐵12 𝐵16 ⎤ ⎡ 𝐵21 𝐵22 𝐵26 ⎥ ⎢ 𝐵16 𝐵26 𝐵66⎦ ⎣ ⎫ ⎧𝜀𝑥 }} {{ 𝜀𝑦 ⎬ ⎨ }} {{ 0⎭ 𝜀𝑧 ⎩ + 𝐷11 𝐷12 𝐷16 ⎤ ⎡ 𝐷21 𝐷22 𝐷26 ⎥ ⎢ 𝐷16 𝐷26 𝐷66⎦ ⎣ {⎧ 𝜅𝑥 }⎫ 𝜅𝑦 𝜅𝑥𝑦⎭}⎬ ⎩{⎨ , (22.88.1) (22.88.2) where 𝐴𝑖𝑗 is the extensional stiffness, 𝐷𝑖𝑗 is the bending stiffness, and 𝐵𝑖𝑗 is the coupling stiffness, which is a null matrix for symmetric lay-ups. The mid-surface strains and 0 and 𝜅𝑖𝑗, respectively. Since these stiffness matrices are curvatures are denoted by 𝜀𝑖𝑗 symmetric, 18 terms are needed per shell element in addition to the shell resultants, which are integrated in time. This is considerably less storage than would typically be required with through thickness integration which requires a minimum of eight history variables per integration point, e.g., if 100 layers are used 800 history variables would be stored. Not only is memory much less for this model, but the CPU time required is also considerably reduced. LS-DYNA Theory Manual Material Models 22.89 Material Model 117-118: Composite Matrix This material is used for modeling the elastic responses of composites where pre- integration, which is done outside of LS-DYNA unlike the lay-up option above, is used to compute the extensional, bending, and coupling stiffness coefficients for use with the Belytschko-Tsay and the assumed strain resultant shell formulations. Since the stresses are not computed in the resultant formulation, the stresses output to the binary databases for the resultant elements are zero. ⎫ The calculation of the force, 𝑁𝑖𝑗, and moment, 𝑀𝑖𝑗, stress resultants is given in 0, and shell curvatures, 𝜅𝑖, as: ⎧ 𝜀𝑥 𝜀𝑦 𝜀𝑧 𝜅𝑥 𝜅𝑦 𝜅𝑥𝑦⎭ 𝐶11 𝐶12 𝐶13 𝐶14 𝐶15 𝐶16 ⎤ ⎡ 𝐶21 𝐶22 𝐶23 𝐶24 𝐶25 𝐶26 ⎥ ⎢ ⎥ ⎢ 𝐶31 𝐶32 𝐶33 𝐶34 𝐶35 𝐶36 ⎥ ⎢ ⎥ ⎢ 𝐶41 𝐶42 𝐶43 𝐶44 𝐶45 𝐶46 ⎥ ⎢ 𝐶51 𝐶52 𝐶53 𝐶54 𝐶55 𝐶56 ⎥ ⎢ 𝐶61 𝐶62 𝐶63 𝐶64 𝐶65 𝐶66⎦ ⎣ terms of the membrane strains, 𝜀𝑖 ⎧ 𝑁𝑥 𝑁𝑦 𝑁𝑥𝑦 𝑀𝑥 𝑀𝑦 𝑀𝑥𝑦⎭ }}}}} }}}}} {{{{{ {{{{{ }}}}} }}}}} {{{{{ {{{{{ (22.89.1) = , ⎫ ⎬ ⎩ ⎨ ⎨ ⎩ ⎬ where 𝐶𝑖𝑗 = 𝐶𝑗𝑖. In this model this symmetric matrix is transformed into the element local system and the coefficients are stored as element history variables. In a variation of this model, *MAT_COMPOSITE_DIRECT, the resultants are already assumed to be given in the element local system which reduces the storage since the 21 coefficients are not stored as history variables as part of the element data. The shell thickness is built into the coefficient matrix and, consequently, within the part ID, which references this material ID, the thickness must be uniform. Material Models LS-DYNA Theory Manual 22.90 Material Model 119: General Nonlinear 6DOF Discrete Beam Catastrophic failure, which is based on displacement resultants, occurs if either of the following inequalities are satisfied: ( 𝑢r tfail 𝑢r ) + ( ) 𝑢s tfail 𝑢s + ( 𝑢t tfail 𝑢t ) + ( 𝜃r tfail 𝜃r ) + ( 𝜃s tfail 𝜃s ) + ( 𝜃t tfail 𝜃t ) − 1. ≥ 0, (22.90.1) ( 𝑢r cfail 𝑢r ) + ( 𝑢s cfail 𝑢s ) + ( 𝑢t cfail 𝑢t ) + ( 𝜃r cfail 𝜃r ) + ( 𝜃s cfail 𝜃s ) + ( 𝜃t cfail 𝜃t ) − 1. ≥ 0. (22.90.2) After failure the discrete element is deleted. If failure is included either the tension failure or the compression failure or both may be used. Unload = 0 loading-unloading curve Unload = 2 Unloading curve Unloading curve Unload = 1 Displacement Displacement Unload = 3 Unloading curve Displacement Displacement Figure 22.90.1. Load and unloading behavior. Umin OFFSET x Umin LS-DYNA Theory Manual Material Models 22.91 Material Model 120: Gurson The Gurson flow function is defined as: 𝛷 = 𝜎M 2 + 2𝑞1𝑓 ∗cosh ( 𝜎Y 3𝑞2𝜎H 2𝜎Y ) − 1 − (𝑞1𝑓 ∗)2 = 0, (22.91.1) where 𝜎M is the equivalent von Mises stress, 𝜎Y is the Yield stress, 𝜎H is the mean hydrostatic stress. The effective void volume fraction is defined as 𝑓 ∗(𝑓 ) = ⎧ {{{ ⎨ {{{ ⎩ 𝑓 ≤ 𝑓c . 𝑓c + 1/𝑞1 − 𝑓c 𝑓F − 𝑓c (𝑓 − 𝑓c) 𝑓 > 𝑓c The growth of void volume fraction is defined as 𝑓 ̇ = 𝑓 ̇ G + 𝑓 ̇ N, where the growth of existing voids is defined as p , 𝑓 ̇ G = (1 − 𝑓 )𝜀̇𝑘𝑘 and the nucleation of new voids is defined as 𝑓 ̇ N = 𝐴𝜀̇p, where 𝐴 = 𝑓N 𝑆N√2π exp (− ( 𝜀p − 𝜀N 𝑆N ) ). (22.91.2) (22.91.3) (22.91.4) (22.91.5) (22.91.6) Material Models LS-DYNA Theory Manual 22.92 Material Model 120: Gurson RCDC The Rc-Dc model is defined as follows. The damage 𝐷 is given by where 𝜀p is the equivalent plastic strain, 𝐷 = ∫ 𝜔1𝜔2𝑑𝜀p, 𝜔1 = ( 1 − 𝛾𝜎m ) , (22.92.1) (22.92.2) is the triaxial stress weighting term and 𝜔2 = (2 − 𝐴D)𝛽, is the asymmetric strain weighting term. In the above 𝜎m is the mean stress and (22.92.3) 𝐴D = min (∣ 𝑆2 𝑆3 ∣ , ∣ 𝑆3 𝑆2 ∣). Fracture is initiated when the accumulation of damage satisfies 𝐷c > 1, where 𝐷c is the critical damage given by 𝐷c = 𝐷0(1 + 𝑏|∇𝐷|λ). (22.92.4) (22.92.5) (22.92.6) LS-DYNA Theory Manual Material Models 22.93 Material Model 124: Tension-Compression Plasticity This is an isotropic elastic-plastic material where a unique yield stress versus plastic strain curve can be defined for compression and tension. Failure can occur based on plastic strain or a minimum time step size. Rate effects are modeled by using the Cowper-Symonds strain rate model. The stress-strain behavior follows one curve in compression and another in tension. The sign of the mean stress determines the state where a positive mean stress (i.e., a negative pressure) is indicative of tension. Two load curves, 𝑓t(𝑝) and 𝑓c(𝑝), are defined, which give the yield stress, 𝜎y, versus effective plastic strain for both the tension and compression regimes. The two pressure values, 𝑝t and 𝑝c, when exceeded, determine if the tension curve or the compressive curve is followed, respectively. If the pressure, 𝑝, falls between these two values, a weighted average of the two curves are used: if − 𝑝t ≤ 𝑝 ≤ 𝑝c {⎧scale = ⎩{⎨ 𝑝c − 𝑝 𝑝c + 𝑝t . (22.93.1) 𝜎y = scale ⋅ 𝑓t(𝑝) + (1 − scale) ⋅ 𝑓c(𝑝) Strain rate is accounted for using the Cowper and Symonds model, which scales the yield stress with the factor p⁄ ) , 1 + ( 𝜀̇ (22.93.2) where 𝜀̇ is the strain rate 𝜀̇ = √𝜀̇𝑖𝑗𝜀̇𝑖𝑗. Material Models LS-DYNA Theory Manual 22.94 Material Model 126: Metallic Honeycomb For efficiency it is strongly recommended that the load curve ID’s: LCA, LCB, LCC, LCS, LCAB, LCBC, and LCCA, contain exactly the same number of points with corresponding strain values on the abscissa. If this recommendation is followed the cost of the table lookup is insignificant. Conversely, the cost increases significantly if the abscissa strain values are not consistent between load curves. The behavior before compaction is orthotropic where the components of the stress tensor are uncoupled, i.e., a component of strain will generate resistance in the local a- direction with no coupling to the local 𝑏 and 𝑐 directions. The elastic modulii vary from their initial values to the fully compacted values linearly with the relative volume: 𝐸𝑎𝑎 = 𝐸𝑎𝑎𝑢 + 𝛽𝑎𝑎(𝐸 − 𝐸𝑎𝑎𝑢), 𝐺𝑎𝑏 = 𝐺𝑎𝑏𝑢 + 𝛽(𝐺 − 𝐺𝑎𝑏𝑢), 𝐸𝑏𝑏 = 𝐸𝑏𝑏𝑢 + 𝛽𝑏𝑏(𝐸 − 𝐸𝑏𝑏𝑢), 𝐺𝑏𝑐 = 𝐺𝑏𝑐𝑢 + 𝛽(𝐺 − 𝐺𝑏𝑐𝑢), 𝐸𝑐𝑐 = 𝐸𝑐𝑐𝑢 + 𝛽𝑐𝑐(𝐸 − 𝐸𝑐𝑐𝑢), 𝐺𝑐𝑎 = 𝐺𝑐𝑎𝑢 + 𝛽(𝐺 − 𝐺𝑐𝑎𝑢), where 𝛽 = max [min ( 1 − 𝑉 1 − 𝑉𝑓 , 1) , 0], and 𝐺 is the elastic shear modulus for the fully compacted honeycomb material 𝐺 = 2(1 + 𝜈) . (22.94.1) (22.94.2) (22.94.3) The relative volume, 𝜈, is defined as the ratio of the current volume over the initial volume, and typically, 𝜈 = 1 at the beginning of a calculation. The load curves define the magnitude of the stress as the material undergoes deformation. The first value in the curve should be less than or equal to zero corresponding to tension and increase to full compaction. Care should be taken when defining the curves so the extrapolated values do not lead to negative yield stresses. At the beginning of the stress update we transform each element’s stresses and strain rates into the local element coordinate system. For the uncompacted material, the trial stress components are updated using the elastic interpolated modulii according to: 𝑛+1trial 𝑛+1trial 𝑛+1trial 𝜎𝑎𝑎 𝜎𝑏𝑏 𝜎𝑐𝑐 = 𝜎𝑎𝑎 = 𝜎𝑏𝑏 = 𝜎𝑐𝑐 𝑛 + 𝐸𝑎𝑎Δ𝜀𝑎𝑎, 𝜎𝑎𝑏 𝑛 + 𝐸𝑏𝑏Δ𝜀𝑏𝑏, 𝜎𝑏𝑐 𝑛 + 𝐸𝑐𝑐Δ𝜀𝑐𝑐, 𝜎𝑐𝑎 𝑛+1trial 𝑛+1trial 𝑛+1trial = 𝜎𝑎𝑏 = 𝜎𝑏𝑐 = 𝜎𝑐𝑎 𝑛 + 2𝐺𝑎𝑏Δ𝜀𝑎𝑏, 𝑛 + 2𝐺𝑏𝑐Δ𝜀𝑏𝑐, 𝑛 + 2𝐺𝑐𝑎Δ𝜀𝑐𝑎, (22.94.4) LS-DYNA Theory Manual Material Models We then independently check each component of the updated stresses to ensure that they do not exceed the permissible values determined from the load curves, e.g., if then 𝑛+1trial ∣𝜎𝑖𝑗 ∣ > 𝜆𝜎𝑖𝑗(𝜀𝑖𝑗), 𝑛+1 = 𝜎𝑖𝑗(𝜀𝑖𝑗) 𝜎𝑖𝑗 𝑛+1trial 𝜆𝜎𝑖𝑗 𝑛+1trial∣ ∣𝜎𝑖𝑗 . (22.94.5) (22.94.6) The components of 𝜎𝑖𝑗(𝜀𝑖𝑗) are defined by load curves. The parameter 𝜆 is either unity or a value taken from the load curve number, LCSR, that defines 𝜆 as a function of strain-rate. Strain-rate is defined here as the Euclidean norm of the deviatoric strain- rate tensor. For fully compacted material we assume that the material behavior is elastic- perfectly plastic and updated the stress components according to: trial = 𝑠𝑖𝑗 𝑠𝑖𝑗 𝑛 + 2𝐺Δ𝜀𝑖𝑗 dev𝑛+1 2⁄ , where the deviatoric strain increment is defined as Δ𝜀𝑖𝑗 dev = Δ𝜀𝑖𝑗 − Δ𝜀𝑘𝑘𝛿𝑖𝑗. (22.94.7) (22.94.8) We now check to see if the yield stress for the fully compacted material is exceeded by comparing trial = ( 𝑠eff 2⁄ trial) trial𝑠𝑖𝑗 𝑠𝑖𝑗 , (22.94.9) the effective trial stress to the yield stress, σy. If the effective trial stress exceeds the yield stress, we simply scale back the stress components to the yield surface 𝑛+1 = 𝑠𝑖𝑗 𝜎y trial 𝑠eff trial. 𝑠𝑖𝑗 We can now update the pressure using the elastic bulk modulus, K 2⁄ 𝑛+1 𝑝𝑛+1 = 𝑝𝑛 − 𝐾Δ𝜀𝑘𝑘 , 3(1 − 2𝜈) 𝐾 = , and obtain the final value for the Cauchy stress 𝑛+1 = 𝑠𝑖𝑗 𝜎𝑖𝑗 𝑛+1 − 𝑝𝑛+1𝛿𝑖𝑗. (22.94.10) (22.94.11) (22.94.12) Material Models LS-DYNA Theory Manual After completing the stress update we transform the stresses back to the global configuration. 22.94.1 Stress Update If LCA < 0, a transversely anisotropic yield surface is obtained where the uniaxial limit stress, 𝜎 y(𝜑, 𝜀vol), can be defined as a function of angle 𝜑 with the strong axis and volumetric strain, 𝜀vol. Elastically, the new material model is assumed to behave exactly as material 126 (with the restriction 𝐸22𝑢 = 𝐸33𝑢 and 𝐺12𝑢 = 𝐺13𝑢), see the LS-DYNA Keyword User’s Manual [Hallquist 2003]. As for the plastic behavior, a natural question that arises is how to define the limit stress for a general multiaxial stress state that reduces to the uniaxial limit stress requirement when the stress is uniaxial. Having given it some thought, we feel that it is most convenient to work with the principal stresses and the corresponding directions to achieve this goal. Assume that the elastic update results in a trial stress 𝜎 trial in the material coordinate system. This stress tensor is diagonalized to obtain the principal stresses trial and the corresponding principal directions 𝐪1, 𝐪2 and 𝐪3 relative to trial, 𝜎2 𝜎1 the material coordinate system. The angle that each direction makes with the strong axis of anisotropy 𝐞1 is given by trial and 𝜎3 Curve extends into negative strain quadrant since LS-DYNA will extrapolate using the two end points. It is important that the extropolation does not extend into the negative stress region. σij unloading and reloading path Strain: -εij Unloading is based on the interpolated Young’s moduli which must provide an unloading tangent that exceeds the loading tangent. Figure 22.94.1. Stress quantity versus strain. Note that the “yield stress” at a strain of zero is nonzero. In the load curve definition the “time” value is the directional strain and the “function” value is the yield stress. LS-DYNA Theory Manual Material Models 𝜑𝑖 = arccos∣𝐪𝑖 ⋅ 𝐞1∣, 𝑖 = 1, 2, 3. (22.94.13) Now a limit stress in the direction of a general multiaxial stress is determined as a convex combination of the uniaxial limit stress in each principal direction 𝜎 Y(𝜎 trial) = 𝑗=1 ∑ 𝜎 Y(𝜙j, 𝜀vol)𝜎𝑗 trial𝜎𝑘 ∑ 𝜎𝑘 𝑘=1 trial𝜎𝑗 trial trial , (22.94.14) Each of the principal stresses is updated as 𝜎𝑖 = 𝜎𝑖 trialmin 1, ⎜⎜⎜⎜⎜⎛ ⎝ 𝜎 Y(𝜎 trial) √∑ 𝜎𝑘 𝑘=1 trial𝜎𝑘 trial , ⎟⎟⎟⎟⎟⎞ ⎠ (22.94.15) and the new stress is transformed back to the material coordinate system3. This stress update is not uniquely defined when the stress tensor possesses multiple eigenvalues, thus the following simple set of rules is applied. If all principal stresses are equal, one of the principal directions is chosen to coincide with the strong axis of anisotropy. If two principal stresses are equal, then one of the directions corresponding to this stress value is chosen perpendicular to the strong axis of anisotropy. 22.94.2 Support for Independent Shear and Hydrostatic Yield Stress Limit The model just described turned out to be weak in shear [Okuda 2003] and there were no means of adding shear resistance without changing the behavior in pure uniaxial compression. We propose the following modification of the model where the user can prescribe the shear and hydrostatic resistance in the material without changing the uniaxial behavior. Assume that the elastic update results in a trial stress 𝜎 trial in the material coordinate system. This stress tensor is diagonalized to obtain the principal stresses trial and the corresponding principal directions 𝐪1, 𝐪2 and 𝐪3 relative to trial, 𝜎2 𝜎1 the material coordinate system. For this discussion we assume that the principal stress values are ordered so that 𝜎1 trial. Two cases need to be treated. trial and 𝜎3 trial ≤ 𝜎2 trial ≤ 𝜎3 3 Since each component of the stress tensor is scaled by the same factor in Equation 19.126.14, the stress is in practice not transformed back but the scaling is performed on the stress in the material coordinate system. Material Models LS-DYNA Theory Manual trial ≤ −𝜎3 If 𝜎1 and consequently 𝜎1 trial then the principal stress value with largest magnitude is 𝜎1 trial ≤ 0. Let trial, 𝜎𝑢 = 𝜎1 𝜎p = trial + max(∣𝜎2 trial∣, ∣𝜎3 trial∣), {−max(∣𝜎2 trial∣, ∣𝜎3 trial∣) + 𝜎2 trial + 𝜎3 trial}, and finally trial∣, ∣𝜎3 trial∣) − 𝜎p 1 = − max(∣𝜎2 𝜎d 2 = 𝜎2 trial − 𝜎p, 𝜎d 3 = 𝜎3 trial − 𝜎p. 𝜎d (22.94.16) (22.94.17) The total stress is the sum of a uniaxial stress represented by 𝜎u, a hydrostatic 3. The angle stress represented by 𝜎p and a deviatoric stress represented by 𝜎d that the direction of 𝜎u makes with the strong axis of anisotropy 𝐞1 is given by 𝜙 = arccos∣𝐪1 ⋅ 𝐞1∣. 2 and 𝜎d 1, 𝜎d Now a limit stress for the general multiaxial stress is determined as a convex combination of the three stress contributions as follows 𝜎 Y(𝜎 trial) Y(𝜙, 𝜀vol)𝜎u 𝜎u 2 + 3√3𝜎p Y(𝜀vol)𝜎p 2 + √2𝜎d = 𝜎u 2 + 3𝜎p 2 + (𝜎d 1)2 + (𝜎d 1)2 + (𝜎d Y(𝜀vol){(𝜎d 2)2 + (𝜎d 3)2 2)2 + (𝜎d 3)2} (22.94.18) . Y(𝜙, εvol) is the prescribed uniaxial stress limit, 𝜎p Here 𝜎u limit and 𝜎d exactly as for the old model. The other two functions are for now written Y(𝜀vol) is the hydrostatic stress Y(𝜀vol) is the stress limit in simple shear. The input for the first of these is Y(𝜀vol) = 𝜎p 𝜎p Y(𝜀vol) = 𝜎d 𝜎d Y + 𝜎 S(𝜀vol), Y + 𝜎 S(𝜀vol), (22.94.19) Y and 𝜎d Y are user prescribed constant stress limits and 𝜎 S is the function where 𝜎p describing the densification of the material when loaded in the direction of the strong material axis. We use the keyword parameters ECCU and GCAU for the new input as follows. • ECCU σd Y, average stress limit (yield) in simple shear. • GCAU σp Y, average stress limit (yield) in hydrostatic compression (pressure). Both of these parameters should be positive. Each of the principal stresses is updated as LS-DYNA Theory Manual Material Models 𝜎𝑖 = 𝜎𝑖 trialmin 1, ⎜⎜⎜⎜⎜⎛ ⎝ 𝜎 Y(𝜎 trial) √∑ 𝜎𝑘 𝑘=1 trial𝜎𝑘 trial , ⎟⎟⎟⎟⎟⎞ ⎠ (22.94.20) and the new stress is transformed back to the material coordinate system. trial ≥ −σ1 If σ3 and consequently σ3 trial then the principal stress value with largest magnitude is σ3 trial ≥ 0. Let trial 𝜎u = 𝜎3 𝜎p = trial − max(∣𝜎2 trial∣, ∣𝜎1 trial∣), {max(∣𝜎2 trial∣, ∣𝜎1 trial∣) + 𝜎2 trial + 𝜎1 trial}, and finally trial − 𝜎p, trial − 𝜎p, 1 = 𝜎1 𝜎d 2 = 𝜎2 𝜎d 3 = max(∣𝜎2 𝜎d trial∣, ∣𝜎1 trial∣) − 𝜎p. (22.94.21) (22.94.22) The angle that the direction of 𝜎u makes with the strong axis of anisotropy 𝐞1 is given by 𝜙 = arccos∣𝐪3 ⋅ 𝐞1∣. The rest of the treatment is the same as for the case when trial. To motivate the model, let us consider three states of stress. trial ≤ −𝜎3 𝜎1 1. 2. 3. For a uniaxial stress 𝜎, we have 𝜎u = 𝜎 and 𝜎p = 𝜎d us to 𝜎 Y(𝜎 trial) = 𝜎u user prescribed uniaxial stress limit. 3 = 0. This leads Y(𝜙, 𝜀vol) and hence the stress level will be limited by the 2 = 𝜎d 1 = 𝜎d For a simple shear 𝜎, we have 𝜎d 𝜎 Y(𝜎 trial) = √2𝜎d scribed shear stress limit. 2 = 𝜎u = 0. Hence Y(𝜀vol) and the stress level will be limited by the user pre- 3 = −𝜎 and 𝜎p = 𝜎d 1 = −𝜎d For a pressure 𝜎, we have 𝜎p = 𝜎 and 𝜎u = 𝜎d 3 = 0. Hence Y(𝜀vol) and the stress level will be limited by the user pre- 2 = 𝜎d 1 = 𝜎d 𝜎 Y(𝜎 trial) = √3𝜎p scribed hydrostatic stress limit. Material Models LS-DYNA Theory Manual 22.95 Material Model 127: Arruda-Boyce Hyperviscoelastic Rubber This material model, described in the paper by Arruda and Boyce [1993], provides a rubber model that is optionally combined with linear viscoelasticity. Rubber is generally considered to be fully incompressible since the bulk modulus greatly exceeds the shear modulus in magnitude; therefore, to model the rubber as an unconstrained material, a hydrostatic work term, 𝑊H(𝐽), is included in the strain energy functional which is a function of the relative volume, 𝐽, [Ogden, 1984]: 𝑊(𝐽1, 𝐽2, 𝐽) = 𝑛𝑘𝜃 [ (𝐽1 − 3) + 19 7000𝑁3 (𝐽1 (𝐽1 20𝑁 4 − 81) + 2 − 9) + 11 1050𝑁2 (𝐽1 519 673750𝑁4 (𝐽1 3 − 27)] 5 − 243)] + 𝑊H(𝐽), (22.95.1) + 𝑛𝑘𝜃 [ 𝐽1 = 𝐼1𝐽−1 𝐽2 = 𝐼2𝐽. 3⁄ , The hydrostatic work term is expressed in terms of the bulk modulus, 𝐾, and 𝐽, as: 𝑊H(𝐽) = (𝐽 − 1)2. (22.95.2) Rate effects are taken into account through linear viscoelasticity by a convolution integral of the form: 𝜎𝑖𝑗 = ∫ 𝑔𝑖𝑗𝑘𝑙 (𝑡 − 𝜏) 𝜕𝜀𝑘𝑙 𝜕𝜏 𝑑𝜏, (22.95.3) or in terms of the second Piola-Kirchhoff stress, 𝑆𝑖𝑗, and Green's strain tensor, 𝐸𝑖𝑗, 𝑆𝑖𝑗 = ∫ 𝐺𝑖𝑗𝑘𝑙 (𝑡 − 𝜏) 𝜕𝐸𝑘𝑙 𝜕𝜏 𝑑𝜏, (22.95.4) where 𝑔𝑖𝑗𝑘𝑙(𝑡 − 𝜏) and 𝐺𝑖𝑗𝑘𝑙(𝑡 − 𝜏) are the relaxation functions for the different stress measures. This stress is added to the stress tensor determined from the strain energy functional. If we wish to include only simple rate effects, the relaxation function is represented by six terms from the Prony series: 𝑔(𝑡) = 𝛼0 + ∑ 𝛼𝑚 𝑚=1 𝑒−𝛽𝑡, (22.95.5) given by, LS-DYNA Theory Manual Material Models 𝑔(𝑡) = ∑ 𝐺𝑖𝑒−𝛽𝑖𝑡 𝑖=1 . (22.95.6) This model is effectively a Maxwell fluid which consists of a dampers and springs in series. We characterize this in the input by shear modulii, 𝐺𝑖, and decay constants, 𝛽𝑖. The viscoelastic behavior is optional and an arbitrary number of terms may be used. Material Models LS-DYNA Theory Manual 22.96 Material Model 128: Heart Tissue This material model provides a tissue model described in the paper by Guccione, McCulloch, and Waldman [1991] The tissue model is described in terms of the energy functional in terms of the Green strain components, 𝐸𝑖𝑗, 𝑊(𝐸, 𝐽) = 𝑄 = 𝑏1𝐸11 (𝑒𝑄 − 1) + 𝑊H(𝐽), 2 + 𝐸33 2 + 𝑏2(𝐸22 2 + 𝐸23 2 + 𝐸32 2 ) + 𝑏3(𝐸12 2 + 𝐸21 2 + 𝐸13 2 + 𝐸31 2 ), (22.96.1) where the hydrostatic work term is in terms of the bulk modulus, 𝐾, and the third invariant 𝐽, as: 𝑊H(𝐽) = (𝐽 − 1)2. (22.96.2) The Green components are modified to eliminate any effects of volumetric work following the procedures of Ogden. LS-DYNA Theory Manual Material Models 22.97 Material Model 129: Isotropic Lung Tissue This material model provides a lung tissue model described in the paper by Vawter [1980]. The material is described by a strain energy functional expressed in terms of the invariants of the Green Strain: 𝑊(𝐼1, 𝐼2) = 𝐴2 = 2𝛥 (𝐼1 + 𝐼2) − 1, 𝑒(𝛼𝐼1 2+𝛽𝐼2) + 12𝐶1 𝛥(1 + 𝐶2) [𝐴(1+𝐶2) − 1], (22.97.1) where the hydrostatic work term is in terms of the bulk modulus, 𝐾, and the third invariant 𝐽, as: 𝑊H(𝐽) = (𝐽 − 1)2, (22.97.2) Rate effects are taken into account through linear viscoelasticity by a convolution integral of the form: 𝜎𝑖𝑗 = ∫ 𝑔𝑖𝑗𝑘𝑙 (𝑡 − 𝜏) 𝜕𝜀𝑘𝑙 𝜕𝜏 𝑑𝜏, (22.97.3) or in terms of the second Piola-Kirchhoff stress, 𝑆𝑖𝑗, and Green's strain tensor, 𝐸𝑖𝑗, 𝑆𝑖𝑗 = ∫ 𝐺𝑖𝑗𝑘𝑙 (𝑡 − 𝜏) 𝜕𝐸𝑘𝑙 𝜕𝜏 𝑑𝜏, (22.97.4) where 𝑔𝑖𝑗𝑘𝑙(𝑡 − 𝜏) and 𝐺𝑖𝑗𝑘𝑙(𝑡 − 𝜏) are the relaxation functions for the different stress measures. This stress is added to the stress tensor determined from the strain energy functional. If we wish to include only simple rate effects, the relaxation function is represented by six terms from the Prony series: given by, 𝑔(𝑡) = 𝛼0 + ∑ 𝛼𝑚 𝑚=1 𝑒−𝛽𝑡, 𝑔(𝑡) = ∑ 𝐺𝑖𝑒−𝛽𝑖𝑡 𝑖=1 . (22.97.5) (22.97.6) This model is effectively a Maxwell fluid which consists of a dampers and springs in series. We characterize this in the input by shear moduli, 𝐺𝑖, and decay Material Models LS-DYNA Theory Manual constants, 𝛽𝑖. The viscoelastic behavior is optional and an arbitrary number of terms may be used. LS-DYNA Theory Manual Material Models 22.98 Material Model 130: Special Orthotropic The in-plane elastic matrix for in-plane plane stress behavior is given by: 𝐂in plane = 𝑄11p 𝑄12p ⎡ 𝑄12p 𝑄22p ⎢ ⎢ ⎢ ⎢ ⎢ ⎣ 𝑄44p 𝑄55p ⎤ ⎥ ⎥ , ⎥ ⎥ ⎥ 𝑄66p⎦ where the terms 𝑄𝑖𝑗p are defined as: 𝑄11p = 𝑄22p = 𝑄12p = 𝐸11p 1 − ν12pν21p 𝐸22p 1 − ν12pν21p ν12pE11p 1 − ν12pν21p , , , 𝑄44p = 𝐺12p, 𝑄55p = 𝐺23p, Q66p = 𝐺31p. The elastic matrix for bending behavior is given by: 𝐂bending = 𝑄11b 𝑄12b ⎡ 𝑄12b 𝑄22b ⎢ ⎣ ⎤ , ⎥ 𝑄44b⎦ (22.98.1) (22.98.2) (22.98.3) where the terms 𝑄𝑖𝑗b are similarly defined. Material Models LS-DYNA Theory Manual 22.99 Material Model 131: Isotropic Smeared Crack The following documentation is taken nearly verbatim from the documentation of that by Lemmen and Meijer [2001]. Three methods are offered to model progressive failure. The maximum principal stress criterion detects failure if the maximum (most tensile) principal stress exceeds 𝜎max. Upon failure, the material can no longer carry stress. The second failure model is the smeared crack model with linear softening stress- strain curve using equivalent uniaxial strains. Failure is assumed to be perpendicular to the principal strain directions. A rotational crack concept is employed in which the crack directions are related to the current directions of principal strain. Therefore crack directions may rotate in time. Principal stresses are expressed as 𝐸̅̅̅̅1 ⎡ ⎢⎢ ⎣ 𝐸̅̅̅̅1𝜀̃1 ⎟⎟⎟⎞ 𝐸̅̅̅̅2𝜀̃2 𝐸̅̅̅̅3𝜀̃3⎠ ⎤ ⎥⎥ 𝐸̅̅̅̅3⎦ 𝜎1 𝜎2 𝜎3⎠ 𝜀̃1 𝜀̃2 𝜀̃3⎠ 𝐸̅̅̅̅2 ⎟⎟⎞ = ⎟⎞ = ⎜⎜⎜⎛ ⎝ ⎜⎜⎛ ⎝ (22.99.1) ⎜⎛ ⎝ , with 𝐸̅̅̅̅1, 𝐸̅̅̅̅2and 𝐸̅̅̅̅3 being secant stiffness in the terms that depend on internal variables. In the model developed for DYCOSS it has been assumed that there is no interaction between the three directions in which case stresses simply follow 𝜎𝑗(𝜀̃𝑗) = ⎧ { { { { { ⎨ { { { { { ⎩ 𝐸𝜀̃𝑗 if 0 ≤ 𝜀̃𝑗 ≤ 𝜀̃𝑗,ini (1 − 𝜀̃𝑗 − 𝜀̃𝑗,ini 𝜀̃𝑗,ult − 𝜀̃𝑗,ini ) 𝜎̅̅̅̅̅ if 𝜀̃𝑗,ini < 𝜀̃𝑗 ≤ 𝜀̃𝑗,ult , (22.99.2) if 𝜀̃𝑗 > 𝜀̃𝑗,ult with 𝜎̅̅̅̅̅ the ultimate stress, 𝜀̃𝑗,ini the damage threshold, and 𝜀̃𝑗,ultthe ultimate strain in 𝑗- direction. The damage threshold is defined as 𝜀̃𝑗,ini = 𝜎̅̅̅̅̅ . (22.99.3) The ultimate strain is obtained by relating the crack growth energy and the dissipated energy ∫ ∫ 𝜎̅̅̅̅̅ 𝑑𝜀̃𝑗,ult 𝑑𝑉 = 𝐺𝐴, (22.99.4) with 𝐺 the energy release rate, 𝑉 the element volume and 𝐴 the area perpendicular to the principal strain direction. The one-point elements in LS-DYNA have a single LS-DYNA Theory Manual Material Models integration point and the integral over the volume may be replaced by the volume. For linear softening it follows 𝜀̃𝑗,ult = 2𝐺𝐴 , 𝑉𝜎̅̅̅̅̅ (22.99.5) The above formulation may be regarded as a damage equivalent to the maximum principle stress criterion. The third model is a damage model presented by Brekelmans et. al. [1991]. Here the Cauchy stress tensor 𝜎 is expressed as 𝜎 = (1 − 𝐷)𝐸𝜀, (22.99.6) where 𝐷 represents the current damage and the factor (1 − 𝐷) is the reduction factor caused by damage. The scalar damage variable is expressed as a function of a so-called damage equivalent strain 𝜀d 𝐷 = 𝐷(𝜀d) = 1 − 𝜀ini(𝜀ult − 𝜀d) 𝜀d(𝜀ult − 𝜀ini) , with ultimate and initial strains as defined by 𝜀d = 𝑘 − 1 2𝑘(1 − 2𝑣) 𝐽1 + 2𝑘 √( 𝑘 − 1 1 − 2𝑣 𝐽1) + 6𝑘 (1 + 𝑣)2 𝐽2, (22.99.7) (22.99.8) where the constant 𝑘 represents the ratio of the strength in tension over the strength in compression 𝑘 = 𝜎ult,tension 𝜎ult,compression , (22.99.9) 𝐽1 and 𝐽2 are the first and the second invariants of the strain tensor representing the volumetric and the deviatoric straining, respectively 𝐽1 = 𝜀𝑖𝑗, ′ 𝜀𝑖𝑗 ′ , 𝐽2 = 𝜀𝑖𝑗 (22.99.10) where 𝜀𝑖𝑗 ′ denotes the deviatoric part of the strain tensor. If the compression and tension strength are equal the dependency on the volumetric strain vanishes in Equation (22.99.8) and failure is shear dominated. If the compressive strength is much larger than the strength in tension, 𝑘 becomes large and the 𝐽1 terms in Equation (22.99.8) dominate the behavior. Material Models LS-DYNA Theory Manual 22.100 Material Model 133: Barlat_YLD2000 The yield condition for this material can be written 𝑓 (𝜎, 𝛼, 𝜀p) = 𝜎eff(𝜎𝑥𝑥 − 2𝛼𝑥𝑥 − 𝛼𝑦𝑦, 𝜎𝑦𝑦 − 2𝛼𝑦𝑦 − 𝛼𝑥𝑥, 𝜎𝑥𝑦 − 𝛼𝑥𝑦) − 𝜎Y t (𝜀p, 𝜀̇p, 𝛽) ≤ 0, (22.100.1) where (𝜑′ + 𝜑′′) 𝜎eff(𝑠𝑥𝑥, 𝑠𝑦𝑦, 𝑠𝑥𝑦) = 𝜑′ = ∣𝑋′1 − 𝑋′2∣𝑎, 𝜑′′ = ∣2𝑋′′1 + 𝑋′′2∣𝑎 + ∣𝑋′′1 + 2𝑋′′2∣𝑎. , ⎟⎞ ⎠ ⎜⎛1 ⎝ The 𝑋′𝑖 and 𝑋′′𝑖 are the eigenvalues of 𝑋′𝑖𝑗 and 𝑋′′𝑖𝑗 and are given by 𝑋′1 = 𝑋′2 = (𝑋′11 + 𝑋′22 + √(𝑋′11 − 𝑋′22)2 + 4𝑋′12 2 ) , (𝑋′11 + 𝑋′22 − √(𝑋′11 − 𝑋′22)2 + 4𝑋′12 2 ), and 𝑋′′1 = 𝑋′′2 = (𝑋′′11 + 𝑋′′22 + √(𝑋′′11 − 𝑋′′22)2 + 4𝑋′′12 2 ) , (𝑋′′11 + 𝑋′′22 − √(𝑋′′11 − 𝑋′′22)2 + 4𝑋′′12 2 ), respectively. The 𝑋′𝑖𝑗 and 𝑋′′𝑖𝑗 are given by4 𝑋′11 ⎟⎟⎟⎞ ⎜⎜⎜⎛ 𝑋′22 𝑋′12⎠ ⎝ 𝑋′′11 𝑋′′22 𝑋′′12⎠ ⎜⎛ ⎝ = ⎜⎜⎜⎛ ⎝ 𝐿′11 𝐿′12 𝐿′21 𝐿′22 𝐿′′11 𝐿′′12 𝐿′′21 𝐿′′22 ⎜⎛ ⎝ ⎟⎞ = ⎟⎟⎟⎞ 𝐿′33⎠ ⎟⎞ 𝐿′′33⎠ ⎜⎛ ⎝ 𝑠𝑥𝑥 ⎟⎞ , 𝑠𝑦𝑦 𝑠𝑥𝑦⎠ 𝑠𝑥𝑥 𝑠𝑦𝑦 𝑠𝑥𝑦⎠ ⎜⎛ ⎝ ⎟⎞, where ⎟⎟⎟⎟⎟⎟⎟⎟⎟⎞ 𝐿′11 𝐿′12 𝐿′21 𝐿′22 𝐿′33⎠ ⎜⎜⎜⎜⎜⎜⎜⎜⎜⎛ ⎝ = −1 0 −1 ⎜⎜⎜⎜⎜⎜⎜⎛ ⎝ ⎟⎟⎟⎟⎟⎟⎟⎞ 3⎠ 𝛼1 𝛼2 𝛼7⎠ ⎟⎞ , ⎜⎛ ⎝ (22.100.2) (22.100.3) (22.100.4) (22.100.5) (22.100.6) LS-DYNA Theory Manual Material Models 𝐿′′11 𝐿′′12 𝐿′′21 𝐿′′22 𝐿′′33⎠ ⎟⎟⎟⎟⎟⎟⎟⎞ ⎜⎜⎜⎜⎜⎜⎜⎛ ⎝ = −2 1 −4 −4 4 −4 −4 −2 8 −2 2 −2 ⎜⎜⎜⎜⎜⎜⎜⎛ ⎝ ⎟⎟⎟⎟⎟⎟⎟⎞ 9⎠ ⎟⎟⎟⎟⎟⎟⎟⎞ 𝛼3 𝛼4 𝛼5 𝛼6 𝛼8⎠ ⎜⎜⎜⎜⎜⎜⎜⎛ ⎝ . where 𝛼1 to 𝛼8 are the parameters that determine the shape of the yield surface. The yield stress is expressed as t (𝜀p, 𝜀̇p, 𝛽) = 𝜎Y 𝜎Y v(𝜀p, 𝜀̇p) + 𝛽(𝜎0 − 𝜎Y v(𝜀p, 𝜀̇p)), (22.100.7) where 𝛽 determines the fraction kinematic hardening and 𝜎0 is the initial yield stress. The yield stress for purely isotropic hardening is given by v(𝜀p, 𝜀̇p) = 𝜎Y(𝜀p) 𝜎Y 1 + { ⎜⎜⎜⎛ ⎝ 𝜀̇p } , ⎟⎟⎟⎞ ⎠ (22.100.8) where 𝐶 and 𝑝 are the Cowper-Symonds material parameters for strain rate effects. The evolution of back stress is given by ⎜⎛∂𝜎Y ∂𝜀p ⎝ ⎜⎛1 + { 𝛼̇ = 𝜆̇𝛽 ⎝ 𝜀̇p } 1/𝑝−1 𝑝𝐶Δ𝑡 𝜀̇p { } 1/p ⎟⎞ + 𝜎Y ⎠ ∂𝜎eff ∂𝑠 ∂𝜎eff ∂𝑠 ⋅ ⎟⎞ ⎠ ∂𝜎eff ∂𝑠 , (22.100.9) where Δ𝑡 is the current time step size and 𝜆̇ is the rate of plastic strain multiplier. For the plastic return algorithms, the gradient of effective stress is computed as ∂𝜎eff ∂𝑠xx ∂𝜎eff ∂𝑠yy ∂𝜎eff ∂𝑠xy ⎠ ⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎞ ⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎛ ⎝ = 𝑎−1 𝑎𝜎eff L′11 L′21 L′12 L′22 ⎜⎜⎜⎛ ⎝ ⎟⎟⎟⎞ L′33⎠ ⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎛ ⎝ 𝜕𝜙′ 𝜕𝑋′11 𝜕𝜙′ 𝜕𝑋′22 𝜕𝜙′ 𝜕𝑋′12⎠ + 𝑎−1 𝑎𝜎eff L′′11 L′′21 L′′12 L′′22 ⎜⎜⎜⎛ ⎝ ⎟⎟⎟⎞ L′′33⎠ ⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎞ ⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎛ ∂𝜙′′ ∂X′′11 ∂𝜙′′ ∂X′′22 ∂𝜙′′ ∂X′′12⎠ ⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎞ with the aid of ⎝ (22.100.10) , Material Models LS-DYNA Theory Manual 𝜕𝜑′ 𝜕𝑋′𝑖𝑗 = 𝑎(𝑋′1 − 𝑋′2)𝑎−1 𝜕(𝑋′1 − 𝑋′2) 𝜕𝑋′𝑖𝑗 , 𝜕𝜑′′ 𝜕𝑋′′𝑖𝑗 = 𝑎∣2𝑋′′1 + 𝑋′′2∣𝑎−1sgn(2𝑋′′1 + 𝑋′′2) 𝑎∣2𝑋′′2 + 𝑋′′1∣𝑎−1sgn(2𝑋′′2 + 𝑋′′1) 𝜕(2𝑋′′1 + 𝑋′′2) 𝜕𝑋′′𝑖𝑗 𝜕(2𝑋′′2 + 𝑋′′1) 𝜕𝑋′′𝑖𝑗 + , and 𝜕(𝑋′1 − 𝑋′2) 𝜕𝑋′11 = 𝑋′11 − 𝑋′22 √(𝑋′11 − 𝑋′22)2 + 4𝑋′12 , 𝜕(𝑋′1 − 𝑋′2) 𝜕𝑋′22 = 𝑋′22 − 𝑋′11 √(𝑋′11 − 𝑋′22)2 + 4𝑋′12 , 𝜕(𝑋′1 − 𝑋′2) 𝜕𝑋′12 = 4𝑋′12 √(𝑋′11 − 𝑋′22)2 + 4𝑋′12 , 𝜕(2𝑋′′1 + 𝑋′′2) 𝜕𝑋′′11 = 𝜕(2𝑋′′1 + 𝑋′′2) 𝜕𝑋′′22 = + 𝑋′′11 − 𝑋′′22 √(𝑋′′11 − 𝑋′′22)2 + 4𝑋′′12 , + 𝑋′′22 − 𝑋′′11 √(𝑋′′11 − 𝑋′′22)2 + 4𝑋′′12 , 𝜕(2𝑋′′1 + 𝑋′′2) 𝜕𝑋′′12 = 2𝑋′′12 √(𝑋′′11 − 𝑋′′22)2 + 4𝑋′′12 , (22.100.11) (22.100.12) (22.100.13) (22.100.14) (22.100.15) (22.100.16) (22.100.17) (22.100.18) 𝜕(2𝑋′′2 + 𝑋′′1) 𝜕𝑋′′11 = − 𝑋′′11 − 𝑋′′22 √(𝑋′′11 − 𝑋′′22)2 + 4𝑋′′12 , (22.100.19) 𝜕(2𝑋′′2 + 𝑋′′1) 𝜕𝑋′′22 = − 𝑋′′22 − 𝑋′′11 √(𝑋′′11 − 𝑋′′22)2 + 4𝑋′′12 , (22.100.20) 𝜕(2𝑋′′2 + 𝑋′′1) 𝜕𝑋′′12 = − 2𝑋′′12 √(𝑋′′11 − 𝑋′′22)2 + 4𝑋′′12 . (22.100.21) The algorithm for the plane stress update as well as the formula for the tangent modulus is given in detail in Section 19.36.1 and is not repeated here. LS-DYNA Theory Manual Material Models 22.100.1 Closest point projection algorithm This section describes shortly the closest point projection algorithm that was implemented to improve accuracy, hence the implicit performance, of the model. The closest point projection comes down to solving the following system of equations 𝑓1 = 𝑡 + 𝐀𝛼 + (𝛔Y t (Δ𝜆) − 𝛔Y t (0))ℎ − 𝛔trial(Δ𝜀33) + 2𝐺Δ𝜆D∇𝜎eff(t) = 0, 𝑓2 = −𝛔eff(t) + 𝛔Y t (Δ𝜆) = 0, 𝑓3 = 𝜎33 trial(Δ𝜀33) + 2𝐺Δ𝜆(∇𝜎eff 1 (t) + ∇𝜎eff 2 (t)) = 0, where ℎ = ∇𝜎eff(𝑡)T𝐁∇𝜎eff(𝑡) 𝐁∇𝜎eff(𝑡), (22.100.22) (22.100.23) (22.100.24) (22.100.25) in terms of the unknown variables 𝐭 (stress), Δε33 (thickness strain increment) and Δ𝜆 (plastic strain increment). In the above 𝐃 = ⎡ ⎢ ⎣ ⎤ , 𝐀 = ⎥ 0.5⎦ ⎡ ⎢ ⎣ ⎤ , 𝐁 = ⎥ 1 ⎦ ⎡ ⎢ ⎣ ⎤ , 𝐻 = ⎥ 0.5⎦ ∂σY ∂εp . (22.100.26) This system of equations is solved using a Newton method with an additional line search for robustness. Using the notation 𝐟 = 𝑓1 ⎤ 𝑓2 ⎥ 𝑓3⎦ ⎡ ⎢ ⎣ , 𝐱 = ⎤, ⎡ Δ𝜆 ⎥ ⎢ Δ𝜀33⎦ ⎣ a Newton step is completed as 𝑥+ = 𝑥− − 𝑠 ( ∂𝑓 ∂𝑥 −1 ) (22.100.27) (22.100.28) for a step size 𝑠 ≤ 1 chosen such that the norm of the objective function is decreasing. The gradient of the objective function is given by ∇𝑓 = ∇𝑓1−β + ∇𝑓β (22.100.29) where ∇f1−β = I + 2𝐺Δ𝜆𝐷∇2𝜎eff ⎡ −(∇𝜎eff)T ⎢⎢ 2𝐺Δ𝜆𝐞T∇2𝛔eff ⎣ 2𝐺𝐷∇𝜎eff −𝐶3 ⎤ ⎥⎥ 2GeT∇σeff C33 ⎦ (22.100.30) Material Models LS-DYNA Theory Manual ∇fβ = ∂h ∂𝑡 ⎡Δ𝜆𝐻 ⎢⎢⎢ 0T ⎣ 𝐻ℎ ⎤ ⎥⎥⎥ 0⎦ and 𝐞 = ⎥⎤, C3 = (K − ⎢⎡ 0⎦ ⎣ 2G ) e, C33 = (K + 4G ), (22.100.31) (22.100.32) 𝐺 and 𝐾 stands for the shear and bulk modulus, respectively. This algorithm requires computation of the effective stress hessian. The derivation of this is quite straightfor- ward but the expression for it is rather long and is hence omitted in this report. LS-DYNA Theory Manual Material Models 22.101 Material Model 134: Viscoelastic Fabric The viscoelastic fabric model is a variation on the general viscoelastic Material Model 76. This model is valid for 3 and 4 node membrane elements only and is strongly recommended for modeling isotropic viscoelastic fabrics where wrinkling may be a problem. For thin fabrics, buckling can result in an inability to support compressive stresses; thus, a flag is included for this option. If bending stresses are important, use a shell formulation with Model 76. Rate effects are taken into account through linear viscoelasticity by a convolution integral of the form: 𝜎𝑖𝑗 = ∫ 𝑔𝑖𝑗𝑘𝑙 (𝑡 − 𝜏) 𝜕𝜀𝑘𝑙 𝜕𝜏 𝑑𝜏, (22.101.1) where 𝑔𝑖𝑗𝑘𝑙(𝑡 − 𝜏) is the relaxation function. If we wish to include only simple rate effects for the deviatoric stresses, the relaxation function is represented by six terms from the Prony series: 𝑔(𝑡) = ∑ 𝐺𝑚 𝑚=1 𝑒−𝛽𝑚𝑡. (22.101.2) We characterize this in the input by shear modulii, 𝐺𝑖, and decay constants, 𝛽𝑖. An arbitrary number of terms, up to 6, may be used when applying the viscoelastic model. For volumetric relaxation, the relaxation function is also represented by the Prony series in terms of bulk modulii: 𝑘(𝑡) = ∑ 𝐾𝑚 𝑚=1 𝑒−𝛽𝑘𝑚𝑡. (22.101.3) Material Models LS-DYNA Theory Manual 22.102 Material Model 139: Modified Force Limited This material model is available for the Belytschko resultant beam element only. Plastic hinges form at the ends of the beam when the moment reaches the plastic moment. The plastic moment versus rotation relationship is specified by the user in the form of a load curve and scale factor. The points of the load curve are (plastic rotation in radians, plastic moment). Both quantities should be positive for all points, with the first point being (zero, initial plastic moment). Within this constraint any form of characteristic may be used, including flat or falling curves. Different load curves and scale factors may be specified at each node and about each of the local s and t axes. Axial collapse occurs when the compressive axial load reaches the collapse load. Collapse load versus collapse deflection is specified in the form of a load curve. The points of the load curve are either (true strain, collapse force) or (change in length, collapse force). Both quantities should be entered as positive for all points, and will be interpreted as compressive. The first point should be (zero, initial collapse load). The collapse load may vary with end moment as well as with deflections. In this case several load-deflection curves are defined, each corresponding to a different end moment. Each load curve should have the same number of points and the same deflection values. The end moment is defined as the average of the absolute moments at each end of the beam and is always positive. Stiffness-proportional damping may be added using the damping factor 𝜆. This is defined as follows: 𝜆 = 2 ∗ 𝜉 , (22.102.1) where 𝜉 is the damping factor at the reference frequency 𝜔 (in radians per second). For example if 1% damping at 2Hz is required 𝜆 = 2 ∗ 0.01 2π ∗ 2 = 0.001592. (22.102.2) If damping is used, a small time step may be required. LS-DYNA does not check this so to avoid instability it may be necessary to control the timestep via a load curve. As a guide, the timestep required for any given element is multiplied by 0.3𝐿/𝑐𝜆 when damping is present (𝐿 = element length, 𝑐 = sound speed). Moment Interaction Plastic hinges can form due to the combined action of moments about the three axes. This facility is activated only when yield moments are defined in the material input. A hinge forms when the following condition is first satisfied. LS-DYNA Theory Manual Material Models ( 𝑀r 𝑀ryield ) + ( 𝑀s 𝑀syield ) + ( 𝑀t 𝑀tyield ) ≥ 1, (22.102.3) where, 𝑀r, 𝑀s, 𝑀t= current moments 𝑀ryield, 𝑀syield, 𝑀tyield= yield moments Note that scale factors for hinge behavior defined in the input will also be applied to the yield moments: for example, 𝑀syield in the above formula is given by the input yield moment about the local axis times the input scale factor for the local s-axis. For strain- softening characteristics, the yield moment should generally be set equal to the initial peak of the moment-rotation load curve. On forming a hinge, upper limit moments are set. These are given by 𝑀rupper = MAX ⎜⎛𝑀r, ⎝ 𝑀ryield ⎟⎞, 2 ⎠ (22.102.4) and similarly for 𝑀s and 𝑀t. Thereafter the plastic moments will be given by: 𝑀rp = min (𝑀rcurve, 𝑀rcurve) and similarly for 𝑠 and 𝑡, where 𝑀rp = current plastic moment 𝑀rcurve = moment taken from load curve at the current rotation scaled according to the scale factor. The effect of this is to provide an upper limit to the moment that can be generated; it represents the softening effect of local buckling at a hinge site. Thus if a member is bent about its local s-axis it will then be weaker in torsion and about its local 𝑡-axis. For moment-softening curves, the effect is to trim off the initial peak (although if the curves subsequently harden, the final hardening will also be trimmed off). It is not possible to make the plastic moment vary with the current axial load, but it is possible to make hinge formation a function of axial load and subsequent plastic moment a function of the moment at the time the hinge formed. This is discussed in the next section. Independent plastic hinge formation In addition to the moment interaction equation, Cards 7 through 18 allow plastic hinges to form independently for the s-axis and t-axis at each end of the beam and also for the torsional axis. A plastic hinge is assumed to form if any component of the current moment exceeds the yield moment as defined by the yield moment vs. axial force curves input on cards 7 and 8. If any of the 5 curves is omitted, a hinge will not form for that component. The curves can be defined for both compressive and tensile axial forces. If the axial force falls outside the range of the curve, the first or last point in the curve will be used. A hinge forming for one component of moment does not affect the other components. Material Models LS-DYNA Theory Manual Upon forming a hinge, the magnitude of that component of moment will not be permitted to exceed the current plastic moment. The current plastic moment is obtained by interpolating between the plastic moment vs. plastic rotation curves input on cards 10, 12, 14, 16, or 18. Curves may be input for up to 8 hinge moments, where the hinge moment is defined as the yield moment at the time that the hinge formed. Curves must be input in order of increasing hinge moment and each curve should have the same plastic rotation values. The first or last curve will be used if the hinge moment falls outside the range of the curves. If no curves are defined, the plastic moment is obtained from the curves on cards 4 through 6. The plastic moment is scaled by the scale factors on lines 4 to 6. A hinge will form if either the independent yield moment is exceeded or if the moment interaction equation is satisfied. If both are true, the plastic moment will be set to the minimum of the interpolated value and 𝑀rp. M8 M7 M6 M5 M4 M3 M2 M1 Strain (or change in length, see AOPT) Figure 22.102.1. The force magnitude is limited by the applied end moment. For an intermediate value of the end moment LS-DYNA interpolates between the curves to determine the allowable force value. LS-DYNA Theory Manual Material Models 22.103 Material Model 141: Rate Sensitive Polymer 𝜀𝑖𝑗 = 𝐷oexp [− ( 𝑍o 3𝐾2 )] 𝑆𝑖𝑗 − 𝛺𝑖𝑗 ⎟⎞, √𝐾2 ⎠ ⎜⎛ ⎝ (22.103.1) where 𝐷o is the maximum inelastic strain rate, 𝑍o is the isotropic initial hardness of material, 𝛺𝑖𝑗 is the internal stress, 𝑆𝑖𝑗 is the deviatoric stress component, and 𝐾2 is defined as follows: 𝐾2 = (𝑆𝑖𝑗 − 𝛺𝑖𝑗)(𝑆𝑖𝑗 − 𝛺𝑖𝑗), (22.103.2) and represent the second invariant of the overstress tensor. The elastic components of the strain are added to the inelastic strain to obtain the total strain. The following relationship defines the internal stress variable rate: 𝛺𝑖𝑗 = 𝑞𝛺m𝜀̇𝑖𝑗 I , I − 𝑞𝛺𝑖𝑗𝜀̇e (22.103.3) where 𝑞 is a material constant, 𝛺m is a material constant that represents the maximum value of the internal stress, and 𝜀̇e I is the effective inelastic strain. Material Models LS-DYNA Theory Manual 22.104 Material Model 142: Transversely Anisotropic Crushable Foam A new material model for low density, transversely isotropic crushable foams, has been developed at DaimlerChrysler by Hirth, Du Bois, and Weimar. Hirth, Du Bois, and Weimar determined that material model 26, MAT_HONEYCOMB, which is commonly used to model foams, can systematically over estimate the stress when it is loaded off-axis. Their new material model overcomes this problem without requiring any additional input. Their new model can possibly replace the MAT_HONEYCOMB material, which is currently used in the frontal offset and side impact barriers. Many polymers used for energy absorption are low density, crushable foams with no noticeable Poisson effect. Frequently manufactured by extrusion, they are transversely isotropic. This class of material is used to enhance automotive safety in low velocity (bumper impact) and medium velocity (interior head impact) applications. These materials require a transversely isotropic, elastoplastic material with a flow rule allowing for large permanent volumetric deformations. The MAT_HONEYCOMB model uses a local coordinate system defined by the user. One of the axes of the local system coincides with the extrusion direction of the honeycomb in the undeformed configuration. As an element deforms, its local coordinate system rotates with its mean rigid body motion. Each of the six stress components is treated independently, and each has its own law relating its flow stress to its plastic strain. The effect of off-axis loading on the MAT_HONEYCOMB model can be estimated by restricting our considerations to plane strain in two dimensions. Our discussion is restricted to the response of the foam before it becomes fully compacted. After compaction, its response is modeled with conventional 𝐽2 plasticity. The model reduces to y (𝜀V), y (𝜀V), y (𝜀V), where 𝜀V is the volumetric strain. For a fixed value of volumetric strain, the individual stress components respond in an elastic-perfectly plastic manner, i.e., the foam doesn’t have any strain hardening. |σ11| ≤ 𝜎11 |𝜎22| ≤ 𝜎22 |𝜎12| ≤ 𝜎12 (22.104.1) In two dimensions, the stress tensor transforms according to [𝜎] = [𝑅(𝜃)]T[𝜎𝜃][𝑅(𝜃)], (22.104.2) LS-DYNA Theory Manual Material Models [𝑅(𝜃)] = [ cos(𝜃) − sin(𝜃) cos(𝜃) sin(𝜃) ], where 𝜃 is the angle of the local coordinate system relative to the global system. For uniaxial loading along the global 1-axis, the stress will be (accounting for the sign of the volume strain), 𝜎11 = {[cos(𝜃)]2𝜎11 y + [sin(𝜃)]2𝜎22 y + 2 ⋅ sin(𝜃)cos(𝜃)𝜎12 y }sgn(𝜀V)}, (22.104.3) assuming the strain is large enough to cause yielding in both directions. y y and 𝜎22 If the shear strength is neglected, 𝜎11 will vary smoothly between 𝜎11 and never exceed the maximum of the two yield stresses. This behavior is intuitively what we would like to see. However, if the value of shear yield stress isn’t zero, 𝜎11 y are equal (a nominally y . To illustrate, if 𝜎11 will be greater than either 𝜎11 isotropic response) the magnitude of the stress is y and 𝜎22 y or 𝜎22 |𝜎11| = 𝜎11 y , y + 2 ⋅ sin(𝜃)cos(𝜃)𝜎12 and achieves a maximum value at 45 degrees of y . y + 𝜎12 |𝜎11| = 𝜎11 (22.104.4) (22.104.5) For cases where there is anisotropy, the maximum occurs at a different angle and will have a different magnitude, but it will exceed the maximum uniaxial yield stress. In fact, a simple calculation using Mohr’s circle shows that the maximum value will be y = 𝜎max (𝜎11 y + 𝜎22 y ) + √(𝜎11 y ) y − 𝜎22 y , + 4𝜎12 (22.104.6) To correct for the systematic overestimation of the off-axis strength by MAT_ HONEYCOMB, MAT_TRANSVERSELY_ISOTROPIC_CRUSHABLE_FOAM has been implemented in LS-DYNA. It uses a single yield surface, calculated dynamically from the six yield stresses specified by the user. The yield surface hardens and softens as a function of the volumetric strain through the yield stress functions. While the cost of the model is higher than for MAT_HONEYCOMB, its superior response off-axis makes it the model of choice for critical applications involving many types of low-density foams. Material Models LS-DYNA Theory Manual 22.105 Material Model 143: Wood Model The wood model is a transversely isotropic material and is available for solid elements. The development of this model was done by Murray [2002], who provided the documentation that follows, under a contract from the FHWA. The general constitutive relation for an orthotropic material, written in terms of the principal material directions [Bodig & Jayne, 1993] is: 𝜎1 ⎤ ⎡ 𝜎2 ⎥ ⎢ 𝜎3 ⎥ ⎢ ⎥ ⎢ 𝜎4 ⎥ ⎢ ⎥ ⎢ 𝜎5 𝜎6⎦ ⎣ = 𝐶11 𝐶12 𝐶13 ⎡ 𝐶21 𝐶22 𝐶23 ⎢ ⎢ 𝐶31 𝐶32 𝐶33 ⎢ ⎢ ⎢ ⎢ ⎣ 2𝐶44 2𝐶55 ⎤ ⎥ ⎥ ⎥ ⎥ ⎥ ⎥ 2𝐶66⎦ = 𝜀1 ⎤ ⎡ 𝜀2 ⎥ ⎢ 𝜀3 ⎥ ⎢ ⎥ ⎢ 𝜀4 ⎥ ⎢ ⎥ ⎢ 𝜀5 𝜀6⎦ ⎣ . (22.105.1) The subscripts 1, 2, and 3 refer to the longitudinal, tangential, and radial, stresses and strains (1 = 11,2 = 22,3 = 33,1 = 11,2 = 22,3 = 33), respectively. The subscripts 4, 5, and 6 are in a shorthand notation that refers to the shearing stresses and strains 4 = 12,5 = 13,6 = 23,4 = 12,5 = 13,6 = 23). As an alternative notation for wood, it is common to substitute L (longitudinal) for 1, T (tangential) for 2, and R (radial) for 3. The components of the constitutive matrix, 𝐶𝑖𝑗, are listed here in terms of the nine independent elastic constants of an orthotropic material: C11 = C22 = C33 = C12 = C13 = , , E11(1 − ν23ν32) E22(1 − ν31ν13) E33(1 − ν12ν21) , (ν21 + ν31ν23)E11 (ν31 + ν21ν32)E11 (ν32 + ν12ν31)E22 C23 = C44 = G12, C55 = G13, C66 = G23, , , , (22.105.2) Δ = 1 − ν12ν21 − ν23ν32 − ν31ν13 − 2ν21ν32ν13. The following identity, relating the dependent (minor Poisson’s ratios ν21, ν31, and ν32) and independent elastic constants, is obtained from symmetry considerations of the constitutive matrix: LS-DYNA Theory Manual Material Models 𝜈𝑖𝑗 𝐸𝑖 = 𝜈𝑗𝑖 𝐸𝑗 for 𝑖, 𝑗 = 1, 2, 3. (22.105.3) One common assumption is that wood materials are transversely isotropic. This means that the properties in the tangential and radial directions are modeled the same, i.e. 𝐸22 = 𝐸33, 𝐺12 = 𝐺13, and 12 = 13. This reduces the number of independent elastic constants to five, 𝐸11, 𝐸22,12, 𝐺12, and 𝐺23. Further, Poisson's ratio in the isotropic plane, 23, is not an independent quantity. It is calculated from the isotropic relation: = (𝐸 − 2𝐺)/2𝐺 where E = 𝐸22 = 𝐸33 and 𝐺 = 𝐺23. Transverse isotropy is a reasonable assumption because the difference between the tangential and radial properties of wood (particularly Southern yellow pine and Douglas fir) is small in comparison with the difference between the tangential and longitudinal properties. The yield surfaces parallel and perpendicular to the grain are formulated from six ultimate strength measurements obtained from uniaxial and pure-shear tests on wood specimens: XT XC YT YC S|| S⊥ Tensile strength parallel to the grain Compressive strength parallel to the grain Tensile strength perpendicular to the grain Compressive strength perpendicular to the grain Shear strength parallel to the grain Shear strength perpendicular to the grain Here 𝑋 and 𝑌 are the strengths parallel and perpendicular to the grain, respectively, and S are the shear strengths. The formulation is based on the work of Hashin [1980]. For the parallel modes, the yield criterion is composed of two terms involving two of the five stress invariants of a transversely isotropic material. These invariants 2 This criterion predicts that the normal and shear stresses are 𝐼1 = 𝜎11 and 𝐼4 = 𝜎12 are mutually weakening, i.e. the presence of shear stress reduces the strength below that measured in uniaxial stress tests. Yielding occurs when 𝑓|| ≥ 0, where: 2 + 𝜎13 𝑓|| = 𝜎11 𝑋2 + (𝜎12 2 ) 2 + 𝜎13 𝑆|| − 1 𝑋 = { 𝑋𝑡 𝑋𝑐 for for 𝜎11 > 0 𝜎11 < 0 . (22.105.4) For the perpendicular modes, the yield criterion is also composed of two terms involving two of the five stress invariants of a transversely isotropic material. These 2 − 𝜎22𝜎33. Yielding occurs when 𝑓 0, where: invariants are 𝐼2 = 22 + 33 and 𝐼3 = 𝜎23 𝑓⊥ = (𝜎22 + 𝜎33)2 𝑌2 + (𝜎23 2 − 𝜎22𝜎33) 𝑆⊥ − 1 𝑌 = { 𝑌t 𝑌c for for 𝜎22 + 𝜎33 > 0 𝜎22 + 𝜎33 < 0 (22.105.5) Material Models LS-DYNA Theory Manual Figure 22.105.1. The yield criteria for wood produces smooth surfaces in stress space. Each yield criterion is plotted in 3D in Figure 22.105.1 in terms of the parallel and perpendicular stresses. Each criterion is a smooth surface (no corners). The plasticity algorithms limit the stress components once the yield criteria in [Murry 2002] are satisfied. This is done by returning the trial elastic stress state back to the yield surface. The stress and strain tensors are partitioned into elastic and plastic parts. Partitioning is done with a return mapping algorithm which enforces the plastic consistency condition. Separate plasticity algorithms are formulated for the parallel and perpendicular modes by enforcing separate consistency conditions. The solution of each consistency condition determines the consistency parameters, and . The Δλ solutions, in turn, determine the stress updates. No input parameters are required. The stresses are readily updated from the total strain increments and the consistency parameters, as follows: 𝑛+1 = 𝜎𝑖𝑗 𝜎̅̅̅̅̅𝑖𝑗 ∗𝑛+1 − 𝐶𝑖𝑗𝑘𝑙Δ𝜆 𝜕𝑓 𝜕𝜎𝑘𝑙 ∣ ∗𝑛+1 = 𝜎𝑖𝑗 𝜎𝑖𝑗 𝑛 + 𝐶𝑖𝑗𝑘𝑙Δ𝜀𝑘𝑙 (22.105.6) (22.105.7) LS-DYNA Theory Manual Material Models ∗are the trial elastic Here 𝑛 denotes the nth time step in the finite element analysis, and 𝜎𝑖𝑗 stress updates calculated from the total strain increments, Δ𝜀𝑖𝑗, prior to application of plasticity. Each normal stress update depends on the consistency parameters and yield surface functions for both the parallel (= || and 𝑓 = 𝑓||) and perpendicular (= and 𝑓 = 𝑓) modes. Each shear stress update depends on just one consistency parameter and yield surface function. If neither parallel nor perpendicular yielding occurs (𝑓|| ∗ < 0) then = 0 and the stress update is trivial: 𝜎̂𝑖𝑗 ∗ < 0 and 𝑓⊥ 𝑛+1 = 𝜎𝑖𝑗 ∗𝑛+1. Wood exhibits pre-peak nonlinearity in compression parallel and perpendicular to the grain. Separate translating yield surface formulations are modeled for the parallel and perpendicular modes, which simulate gradual changes in moduli. Each initial yield surface hardens until it coincides with the ultimate yield surface. The initial location of the yield surface determines the onset of plasticity. The rate of translation determines the extent of the nonlinearity. For each mode (parallel and perpendicular), the user inputs two parameters: the initial yield surface location in uniaxial compression, 𝑁, and the rate of translation, 𝑐. Say the user wants pre-peak nonlinearity to initiate at 70% of the peak strength. The user will input 𝑁 = 0.3 so that 1 − 𝑁 = 0.7. If the user wants to harden rapidly, then a large value of 𝑐 is input, like 𝑐 = 1 msec. If the user wants to harden gradually, then a small value of 𝑐 is input, like 𝑐 = 0.2 msec. The state variable that defines the translation of the yield surface is known as the back stress, and is denoted by 𝑖𝑗. Hardening is modeled in compression, but not shear, so the only back stress required for the parallel modes is 11. The value of the back stress is 11 = 0 upon initial yield and 11 = −𝑁|| 𝑋𝑐 at ultimate yield (in uniaxial compression). The maximum back stress occurs at ultimate yield and is equal to the total translation of the yield surface in stress space. The back stress components required for the perpendicular modes are 22 and 33. The value of the backstress sum XT Tension -(1-NII)Xc -xc Initial Yield Surface Ultimate Yield Surace Compression SII Square root of parallel shear invariant Xc (1-NII)Xc | | Ultimate Yield Strength CII large CII small Increasing Rate of Translation NIIXc Initial Yield Strength Strain (a) Initial and ultimate yield surfaces (b) Stress-strain behavior Figure 22.105.2. Pre-peak nonlinearity in compression is modeled with translating yield surfaces that allow the user to specify the hardening response. Material Models LS-DYNA Theory Manual is 22 + 33 = 0 upon initial yield and 22 + 33 = −𝑁 𝑌𝑐 at ultimate yield (biaxial compression without shear). Separate damage formulations are modeled for the parallel and perpendicular modes. These formulations are loosely based on the work of Simo and Ju [1987]. If failure occurs in the parallel modes, then all six stress components are degraded uniformly. This is because parallel failure is catastrophic, and will render the wood useless. If failure occurs in the perpendicular modes, then only the perpendicular stress components are degraded. This is because perpendicular failure is not catastrophic: we expect the wood to continue to carry load in the parallel direction. Based on these assumptions, the following degradation model is implemented: 𝑑m = max(𝑑(𝜏||), 𝑑(𝜏⊥)) , 𝑑|| = 𝑑(𝜏||), 𝜎11 = (1 − 𝑑||)𝜎̅̅̅̅̅11, 𝜎22 = (1 − 𝑑m)𝜎̅̅̅̅̅22, 𝜎33 = (1 − 𝑑m)𝜎̅̅̅̅̅33, σ12 = (1 − 𝑑||)𝜎̅̅̅̅̅12, 𝜎13 = (1 − 𝑑||)𝜎̅̅̅̅̅13, 𝜎23 = (1 − 𝑑m)𝜎̅̅̅̅̅23. (22.105.8) Here, each scalar damage parameter, 𝑑, transforms the stress tensor associated with the undamaged state, 𝜎̅̅̅̅̅𝑖𝑗, into the stress tensor associated with the damaged state, 𝑖𝑗. The stress tensor 𝜎̅̅̅̅̅𝑖𝑗 is calculated by the plasticity algorithm prior to application of the damage model. Each damage parameter ranges from zero for no damage and approaches unity for maximum damage. Thus 1 − 𝑑 is a reduction factor associated with the amount of damage. Each damage parameter evolves as a function of a strain energy-type term. Mesh size dependency is regulated via a length scale based on the element size (cube root of volume). Damage-based softening is brittle in tension, less brittle in shear, and ductile (no softening) in compression, as demonstrated in Figure 22.105.1. Element erosion occurs when an element fails in the parallel mode, and the parallel damage parameter exceeds 𝑑|| = 0.99. Elements do not automatically erode when an element fails in the perpendicular mode. A flag is available, which, when set, allows elements to erode when the perpendicular damage parameter exceeds 𝑑 = 0.99. Setting this flag is not recommended unless excessive perpendicular damage is causing computational difficulties. LS-DYNA Theory Manual Material Models (a) Tensile softening. (b) Shear softening. (c) Compressive yielding. Figure 19.143.3. Softening response modeled for parallel modes of Southern yellow pine. Data available in the literature for pine [Reid & Peng, 1997] indicates that dynamic strength enhancement is more pronounced in the perpendicular direction than in the parallel direction. Therefore, separate rate effects formulations are modeled for Material Models LS-DYNA Theory Manual the parallel and perpendicular modes. The formulations increase strength with increasing strain rate by expanding each yield surface: 𝜎11 = 𝑋 + 𝐸11𝜀̇ 𝜂|| 𝜎22 = 𝑌 + 𝐸22𝜀̇ 𝜂⊥ Parallel Perpendicular . (22.105.9) Here 𝑋 and 𝑌 are the static strengths, 11 and 22 are the dynamic strengths, and 𝐸11𝜀̇ 𝜂|| and 𝐸22𝜀̇ 𝜂⊥ are the excess stress components. The excess stress components depend on the value of the fluidity parameter, , as well as the stiffness and strain rate. The user inputs two values, 0 and 𝑛, to define each fluidity parameter: 𝜂|| = 𝜂⊥ = 𝜂0|| 𝜀̇𝑛|| 𝜂0⊥ 𝜀̇𝑛⊥ , . (22.105.10) The two parameter formulation [Murray, 1997] allows the user to model a nonlinear variation in dynamic strength with strain rate. Setting 𝑛 = 0 allows the user to model a linear variation in dynamic strength with strain rate. LS-DYNA Theory Manual Material Models 22.106 Material Model 144: Pitzer Crushable Foam The logarithmic volumetric strain is defined in terms of the relative volume, 𝑉, as: In defining the curves the stress and strain pairs should be positive values starting with a volumetric strain value of zero. 𝛾 = −ln(𝑉). (22.106.1) Viscous damping in the model follows an implementation identical to that of material type 57. Material Models LS-DYNA Theory Manual 22.107 Material Model 147: FHWA Soil Model A brief discussion of the FHWA soil model is given. The elastic properties of the soil are isotropic. The implementation of the modified Mohr-Coulomb plasticity surface is based on the work of Abbo and Sloan [1995]. The model is extended to include excess pore water effects, strain softening, kinematic hardening, strain rate effects, and element deletion. The modified yield surface is a hyperbola fitted to the Mohr-Coulomb surface. At the crossing of the pressure axis (zero shear strength) the modified surface is a smooth surface and it is perpendicular to the pressure axis. The yield surface is given as 𝐹 = −𝑃sin𝜙 + √𝐽2𝐾(𝜃)2 + AHYP2sin2𝜙 − 𝑐cos𝜙 = 0, (22.107.1) where 𝑃 is the pressure, 𝜙 is the internal friction angle, 𝐾(𝜃) is a function of the angle in 𝐹 = −𝑃sin𝜑 + √𝐽2𝐾(𝜃)2 + AHYP2sin2𝜑 − 𝑐cos𝜑 = 0, (22.107.2) deviatoric plane, √𝐽2 is the square root of the second invariant of the stress deviator, 𝑐 is the amount of cohesion and , cos3𝜃 = 3√3𝐽3 2𝐽2 J3 is the third invariant of the stress deviator, AHYP is a parameter for determining how close to the standard Mohr-Coulomb yield surface the modified surface is fitted. If the user defined parameter, AHYP, is input as zero, the standard Mohr-Coulomb surface is recovered. The parameter aℎypshould be set close to zero, based on numerical considerations, but always less than 𝑐 cot𝜙. It is best not to set the cohesion, 𝑐, to very small values as this causes excessive iterations in the plasticity routines. (22.107.3) To generalize the shape in the deviatoric plane, we have changed the standard Mohr- Coulomb 𝐾(𝜃) function to a function used by Klisinski [1985] 𝐾(𝜃) = 4(1 − 𝑒2)cos2𝜃 + (2𝑒 − 1)2 2(1 − 𝑒2)cos𝜃 + (2𝑒 − 1)[4(1 − 𝑒2)cos2𝜃 + 5𝑒2 − 4𝑒] , (22.107.4) where 𝑒 is a material parameter describing the ratio of triaxial extension strength to triaxial compression strength. If e is set equal to 1, then a circular cone surface is formed. If 𝑒 is set to 0.55, then a triangular surface is found, 𝐾(𝜃) is defined for 0.5 < 𝑒 ≤ 1.0. LS-DYNA Theory Manual Material Models Figure 22.107.1. Pressure versus volumetric strain showing the effects of D1 parameter. To simulate non-linear strain hardening behavior the friction, angle 𝜙 is increased as a function of the effective plastic strain, Δ𝜑 = 𝐸t (1 − 𝜑 − 𝜑init 𝐴𝑛𝜑max ) Δ𝜀eff plas. (22.107.5) where 𝜀eff plas is the effective plastic strain. 𝐴𝑛 is the fraction of the peak strength internal friction angle where nonlinear behavior begins, 0 < 𝐴𝑛 ≤ 1. The input parameter 𝐸𝑡 determines the rate of the nonlinear hardening. To simulate the effects of moisture and air voids including excess pore water pressure, both the elastic and plastic behaviors can be modified. The bulk modulus is 𝐾 = 𝐾𝑖 1 + 𝐾𝑖𝐷1𝑛cur . (22.107.6) where 𝐾𝑖 = initial bulk modulus 𝑛cur = current porosity = Max[0, (𝑤 − 𝜀v)] 𝑤 = volumetric strain corresponding to the volume of air voids = 𝑛(1 − 𝑆) 𝜀v = total volumetric strain 𝐷1 = material constant controlling the stiffness before the air voids are collapsed 𝑛 = porosity of the soil = 1 + 𝑒 Material Models LS-DYNA Theory Manual Figure 22.107.2. The effect on pressure due to pore water pressure. 𝑒 = void ratio = γsp(1 + mc) − 1 𝑆 = degree of saturation = 𝜌𝑚c 𝑛(1 + 𝑚c) and 𝜌, 𝛾, 𝑚c are the soil density, specific gravity, and moisture content, respectively. Figure 22.107.1 shows the effect of the 𝐷1 parameter on the pressure-volumetric strain relationship (bulk modulus). The bulk modulus will always be a monotonically increasing value, i.e., 𝐾𝑗+1 = 𝐾𝑖 1 + 𝐾𝑖𝐷1𝑛cur 𝐾𝑗 ⎧ { ⎨ { ⎩ if 𝜀𝑣 𝑗+1 > 𝜀𝑣𝑗 . if 𝜀𝑣 𝑗+1 ≤ 𝜀𝑣𝑗 (22.107.7) Note that the model is following the standard practice of assuming compressive stresses and strains are positive. If the input parameter 𝐷1 is zero, then the standard linear elastic bulk modulus behavior is used. To simulate the loss of shear strength due to excess pore water effects, the model uses a standard soil mechanics technique [Holtz and Kovacs, 1981] of reducing the total pressure, 𝑃, by the excess pore water pressure, 𝑢, to get an “ effective pressure”, 𝑃′; therefore, 𝑃′ = 𝑃 − 𝑢. (22.107.8) Figure 22.107.2 shows pore water pressure will affect the algorithm for the plasticity surface. The excess pore water pressure reduces the total pressure, which will LS-DYNA Theory Manual Material Models lower the shear strength, √𝐽2. A large excess pore water pressure can cause the effective pressure to become zero. To calculate the pore water pressure, 𝑢, the model uses an equation similar to the equation used for the moisture effects on the bulk modulus. 𝑢 = 𝐾sk 1 + 𝐾sk𝐷2𝑛cur 𝜀𝑣, (22.107.9) where 𝐾sk = bulk modulus for soil without air voids (skeletal bulk modulus) 𝑛cur = current porosity = Max[0, (𝑤 − 𝜀𝑣)] 𝑤 = volumetric strain corresponding to the volume of air voids = 𝑛(1 − 𝑆) 𝜀v = total volumetric strain 𝐷2 = material constant controlling the pore water pressure before the air voids are collapsed to 𝐷2 ≥ 0 𝑛 = porosity of the soil = 𝑒 = void ratio = 1 + 𝑒 γsp(1 + mc) 𝑆 = degree of saturation = − 1 𝜌𝑚c 𝑛(1 + 𝑚c) and 𝜌, 𝛾, 𝑚c are the soil density, specific gravity, and moisture content, respectively. The pore water pressure will not be allowed to become negative, 𝑢 ≥ 0. Figure 22.107.3 is a plot of the pore pressure versus volumetric strain for different parameter values. With the 𝐷2 parameter set relatively high compared to 𝐾sk there is no pore pressure until the volumetric strain is greater than the strains associated with the air voids. However, as 𝐷2 is lowered, the pore pressure starts to increase before the air voids are totally collapsed. The 𝐾sk parameter affects the slope of the post-void collapse pressure - volumetric behavior. Material Models LS-DYNA Theory Manual The parameter 𝐷2 can be found from Skempton pore water pressure parameter 𝐵, where 𝐵 is defined as [Holtz and Kovacs, 1981]: 𝐵 = 𝐷2 = , 1 + 𝑛 𝐾sk 𝐾v 1 − 𝐵 𝐵𝐾sk[𝑛(1 − 𝑆)] . (22.107.10) To simulate strain softening behavior the FHWA soil model uses a continuum damage algorithm. The strain-based damage algorithm is based on the work of J. W. Ju and J. C. Simo [1987, 1989]. They proposed a strain based damage criterion, which is uncoupled from the plasticity algorithm. For the damage criterion, 𝜉 = − 𝐾𝑖 ∫ 𝑃̅̅̅̅̅𝑑𝜀pv, (22.107.11) where 𝑃̅̅̅̅̅ is the pressure and 𝜀pv is the plastic volumetric strain, the damaged stress is found from the undamaged stresses. 𝜎 = (1 − 𝑑)𝜎̅̅̅̅̅, (22.107.12) where 𝑑 is the isotropic damage parameter. The damage parameter is found at step 𝑗 + 1 as: Figure 22.107.3. The effects of 𝐷2 and 𝐾sk parameters on pore water pressure. LS-DYNA Theory Manual Material Models 𝑑𝑗+1 = 𝑑𝑗 if 𝜉𝑗+1 ≤ 𝑟𝑗 𝑑𝑗+1 = 𝜉𝑗+1 − 𝜉0 𝛼 − 𝜉0 if 𝜉𝑗+1 > 𝑟𝑗 , (22.107.13) where 𝑟t is a damage threshold surface, 𝑟𝑗+1 = max{𝑟𝑗, 𝜉𝑗+1), and 𝜉0 = 𝑟0 (DINT). The mesh sensitivity parameter, 𝛼, will be described below. Typically, the damage, 𝑑, varies from 0 to a maximum of 1. However, some soils can have a residual strength that is pressure dependent. The residual strength is represented by 𝜙res, the minimum internal friction angle. The maximum damage allowed is related to the internal friction angle of residual strength by: 𝑑max = sin𝜙 − sin𝜙res sin𝜙 , (22.107.14) If 𝜙res > 0, then 𝑑max, the maximum damage, will not reach 1, and the soil will have some residual strength. When material models include strain softening, special techniques must be used to prevent mesh sensitivity. Mesh sensitivity is the tendency of the finite element model/analysis to produce significantly different results as the element size is reduced. The mesh sensitivity occurs because the softening in the model concentrates in one element. As the element size is reduced the failure becomes localized in smaller volumes, which causes less energy to be dissipated by the softening leading to instabilities or at least mesh sensitive behavior. To eliminate or reduce the effects of strain softening mesh sensitivity, the softening parameter, α (the strain at full damage), must be modified as the element size changes. The FHWA soil model uses an input parameter, “void formation”, 𝐺f, that is like fracture energy material property for metals. The void formation parameter is the area under the softening region of the pressure volumetric strain curve times the cube root of the element volume, 𝑉 3. 𝐺f = 𝑉 3 ∫ 𝑃 𝜉0 𝑑𝜀v = 𝑃peak(𝛼 − 𝜉0)𝑉 , (22.107.15) with 𝜉0, the volumetric strain at peak pressure (strain at initial damage, DINT). Then 𝛼 can be found as a function of the volume of the element 𝑉: 𝛼 = 2𝐺f 3⁄ 𝐾𝜉0𝑉 + 𝜉0. (22.107.16) Material Models LS-DYNA Theory Manual If 𝐺f is made very small relative to 𝐾𝜉0𝑉 3⁄ , then the softening behavior will be brittle. Strain-rate enhanced strength is simulated by a two-parameter Devaut-Lions viscoplastic update algorithm, developed by Murray [1997]. This algorithm interpolates between the elastic trial stress (beyond the plasticity surface) and the inviscid stress. The inviscid stresses (𝜎̅̅̅̅̅) are on the plasticity surface. Δ𝑡+𝜂, and 𝜂 = ( 𝜎̅̅̅̅̅vp = (1 − 𝜍)𝜎̅̅̅̅̅ + 𝜍𝜎̅̅̅̅̅trial, 𝛾r 𝜀̇ )(𝑣𝑛−1)/𝑣𝑛. where 𝜍 = (22.107.17) As 𝜁 approaches 1, then the viscoplastic stress becomes the elastic trial stress. Setting the input value 𝛾r = 0 eliminates any strain-rate enhanced strength effects. The model allows element deletion, if needed. As the strain softening (damage) increases, the effective stiffness of the element can get very small, causing severe element distortion and hourglassing. The element can be “deleted” to remedy this behavior. There are two input parameters that affect the point of element deletion. DAMLEV is the damage threshold where element deletion will be considered. EPSPRMAX is the maximum principal strain where element will be deleted. Therefore, 𝑑 ≥ DAMLEV and 𝜀prmax > EPSPRMAX, (22.107.18) for element deletion to occur. If DAMLEV is set to zero, there is no element deletion. Care must be taken when employing element deletion to assure that the internal forces are very small (element stiffness is zero) or significant errors can be introduced into the analysis. The keyword option, NEBRASKA, gives the soil parameters used to validate the material model with experiments performed at University of Nebraska at Lincoln. The units for this default inputs are milliseconds, kilograms, and millimeters. There are no required input parameters except material id (MID). If different units are desired the unit conversion factors that need to multiply the default parameters can be input. LS-DYNA Theory Manual Material Models 22.108 Material Model 154: Deshpande-Fleck Foam The equivalent stress, 𝜎̂ , is given by: 𝛷 = 𝜎̂ − 𝜎Y, 𝜎̂ 2 = 2 + 𝛼2𝜎m 𝜎VM 1 + (𝛼/3)2 , where, 𝜎VM, is the von Mises effective stress, 𝜎VM = √ 𝛔dev: 𝛔dev, and, 𝜎mand 𝛔dev, is the mean and deviatoric stress 𝜎m = tr(𝛔) 𝛔dev = 𝛔 − σm𝐈. The yield stress 𝜎Y can be expressed as 𝜎Y = 𝜎p + 𝛾 𝜀̂ 𝜀D + 𝛼2 ( 1 − (𝜀̂/𝜀D)𝛽 ), (22.108.1) (22.108.2) (22.108.3) (22.108.4) (22.108.5) Here, 𝜎p, 𝛼2, 𝛾 and 𝛽 are material parameters. The densification strain, 𝜀D, is defined as 𝜌f 𝜌f0 𝜀D = −ln ( (22.108.6) ), where 𝜌f is the foam density and 𝜌f0 is the density of the virgin material. Material Models LS-DYNA Theory Manual 22.109 Material Model 156: Muscle The material behavior of from *MAT_SPRING_MUSCLE, the spring muscle model and treated here as a standard material. The initial length of muscle is calculated automatically. The force, relative length and shortening velocity are replaced by stress, strain and strain rate. A new parallel damping element is added. the muscle model adapted is The strain and normalized strain rate are defined respectively as − 1 = 𝐿 − 1 𝑙𝑜 𝜀 = 𝜀̇ = 𝑙 ̇ 𝑙o 𝜀̇max = 𝑉M 𝑙𝑜 ∗ (SRM ∗ SFR) = 𝑉M (𝑙𝑜 ∗ SRM) ∗ SFR = 𝑉M 𝑉max ∗ SFR = 𝑉, (22.109.1) where 𝑙𝑜 is the original muscle length. From the relation above, it is known: 𝑙𝑜 = 𝑙0 1 + 𝜀0 , (22.109.2) where 𝜀0 = SNO; 𝑙0 = muscle length at time 0. Stress of Contractile Element is: 𝜎1 = 𝜎max 𝑎(𝑡)𝑓 (𝜀) 𝑔(𝜀̇), (22.109.3) where 𝜎max =PIS; 𝑎(𝑡) =ALM; 𝑓 (𝜀) =SVS; 𝑔(𝜀̇) =SVR. Stress of Passive Element is: 𝜎2 = 𝜎maxℎ(ε). (22.109.4) For exponential relationship: ℎ(ε) = ⎧ {{{{{ {{{{{ ⎨ ⎩ 𝜀 ≤ 0 exp(𝑐) − 1 [ exp ( 𝑐𝜀 𝐿max ) − 1 ] 𝜀 > 0 𝑐 ≠ 0 (22.109.5) ⁄ 𝜀 𝐿max 𝜀 > 0 𝑐 = 0 where 𝐿max = 1 + SSM; and 𝑐 =CER. Stress of Damping Element is: Total Stress is: 𝜎3 = 𝐷𝜀̇max𝜀̇ 𝜎 = 𝜎1 + 𝜎2 + 𝜎3. (22.109.6) (22.109.7) LS-DYNA Theory Manual Material Models 22.110 Material Model 158: Rate Sensitive Composite Fabric See material type 58, Laminated Composite Fabric, for the treatment of the composite material. Rate effects are taken into account through a Maxwell model using linear viscoelasticity by a convolution integral of the form: 𝜎𝑖𝑗 = ∫ 𝑔𝑖𝑗𝑘𝑙(𝑡 − 𝜏) 𝜕𝜀𝑘𝑙 𝜕𝜏 𝑑𝜏 , (22.110.1) where 𝑔𝑖𝑗𝑘𝑙(𝑡 − 𝜏) is the relaxation function for different stress measures. This stress is added to the stress tensor determined from the strain energy functional. Since we wish to include only simple rate effects, the relaxation function is represented by six terms from the Prony series: 𝑔(𝑡) = ∑ 𝐺𝑚𝑒−𝛽𝑚𝑡 𝑚=1 . (22.110.2) We characterize this in the input by the shear moduli, 𝐺𝑖, and the decay constants, 𝛽𝑖. An arbitrary number of terms, not exceeding 6, may be used when applying the viscoelastic model. The composite failure is not directly affected by the presence of the viscous stress tensor. Material Models LS-DYNA Theory Manual 22.111 Material Model 159: Continuous Surface Cap Model This is a cap model with a smooth intersection between the shear yield surface and hardening cap, as shown in Figure 22.111.1. The initial damage surface coincides with the yield surface. Rate effects are modeled with viscoplasticity. See [Murray 2007] for a more complete description of the material model. Stress Invariants. The yield surface is formulated in terms of three stress invariants: 𝐽1 is the first invariant of the stress tensor, 𝐽′2 is the second invariant of the deviatoric stress tensor, and 𝐽′3 is the third invariant of the deviatoric stress tensor. The invariants are defined in terms of the deviatoric stress tensor, 𝑆𝑖𝑗 and pressure, 𝑃, as follows: 𝐽1 = 3𝑃, 𝐽′ 2 = 𝑆𝑖𝑗𝑆𝑖𝑗, 𝐽′ 3 = 𝑆𝑖𝑗𝑆𝑗𝑘𝑆𝑘𝑖. (22.111.1) Plasticity Surface. The three invariant yield function is based on these three invariants, and the cap hardening parameter, 𝑘, as follows: 𝑓 (𝐽1, 𝐽′2, 𝐽′3, 𝜅) = 𝐽′2 − ℜ2𝐹f (22.111.2) Here 𝐹f is the shear failure surface, 𝐹c is the hardening cap, and ℜ is the Rubin three- invariant reduction factor. The cap hardening parameter 𝜅 is the value of the pressure invariant at the intersection of the cap and shear surfaces. 2𝐹c. Trial elastic stress invariants are temporarily updated via the trial elastic stress ′𝑇. Elastic stress states are modeled when tensor, 𝜎 T. These are denoted 𝐽1 ′𝑇 and 𝐽3 𝑇 , 𝐽2 Figure 22.111.1. General Shape of the concrete model yield surface in two- dimensions. LS-DYNA Theory Manual Material Models 𝑓 (𝐽1, 𝐽′2, 𝐽′3, 𝜅𝑇) < 0. Elastic-plastic stress states are modeled when 𝑓 (𝐽1, 𝐽′2, 𝐽′3, 𝜅𝑇) > 0. In this case, the plasticity algorithm returns the stress state to the yield surface such that 𝑃, 𝜅𝑃) = 0. This is accomplished by enforcing the plastic consistency 𝑓 (𝐽1 condition with associated flow. 𝑃, 𝐽′3 𝑃, 𝐽′2 Shear Failure Surface. The strength of concrete is modeled by the shear surface in the tensile and low confining pressure regimes: 𝐹f(𝐽1) = 𝛼 − 𝜆𝑒−𝛽𝐽1 + 𝜃𝐽1. (22.111.3) Here the values of 𝛼, 𝛽, 𝜆, and 𝜃 are selected by fitting the model surface to strength measurements from triaxial compression (txc) tests conducted on plain concrete cylinders. ′ (principal stress Rubin Scaling Function. Concrete fails at lower values of √3𝐽2 difference) for triaxial extension (txe) and torsion (tor) tests than it does for txc tests conducted at the same pressure. The Rubin scaling function ℜ determines the strength of concrete for any state of stress relative to the strength for txc, via ℜ𝐹𝑓 . Strength in torsion is modeled as 𝑄1𝐹f. Strength in txe is modeled as 𝑄2𝐹f, where: 𝑄1 = 𝛼1 − 𝜆1𝑒−𝛽1𝐽1 + 𝜃1𝐽1, 𝑄2 = 𝛼2 − 𝜆2𝑒−𝛽2𝐽1 + 𝜃2𝐽1. (22.111.4) Cap Hardening Surface. The strength of concrete is modeled by a combination of the cap and shear surfaces in the low to high confining pressure regimes. The cap is used to model plastic volume change related to pore collapse (although the pores are not explicitly modeled). The isotropic hardening cap is a two-part function that is either unity or an ellipse: 𝐹c( 𝐽1, 𝜅 ) = 1 − [𝐽1 − 𝐿 (𝜅)][|𝐽1 − 𝐿(𝜅)| + 𝐽1 − 𝐿(𝜅)] 2[𝑋(𝜅) − 𝐿 (𝜅)] 2 , (22.111.5) where 𝐿(𝜅) is defined as: L(κ) = { if 𝜅 > 𝜅0 𝜅0 otherwise . (22.111.6) The equation for 𝐹c is equal to unity for 𝐽1 𝐿(𝜅). It describes the ellipse for 𝐽1 > 𝐿(𝜅). The intersection of the shear surface and the cap is at 𝐽1 = 𝜅. 𝜅0 is the value of 𝐽1 at the initial intersection of the cap and shear surfaces before hardening is engaged (before the cap moves). The equation for 𝐿(𝜅) restrains the cap from retracting past its initial location at 𝜅0. The intersection of the cap with the 𝐽1 axis is at 𝐽1 = 𝑋(𝜅). This intersection depends upon the cap ellipticity ratio 𝑅, where 𝑅 is the ratio of its major to minor axes: 𝑋(𝜅) = 𝐿(𝜅) + 𝑅𝐹f(𝐿(𝜅)). (22.111.7) Material Models LS-DYNA Theory Manual The cap expands (𝑋(𝜅) The cap moves to simulate plastic volume change. and 𝜅 increase) to simulate plastic volume compaction. The cap contracts (𝑋(𝜅) and 𝜅 decrease) to simulate plastic volume expansion, called dilation. The motion (expansion and contraction) of the cap is based upon the hardening rule: p = 𝑊(1 − 𝑒−𝐷1(𝑋−𝑋0)−𝐷2(𝑋−𝑋0)2 𝜀𝑣 (22.111.8) p the plastic volume strain, 𝑊 is the maximum plastic volume strain, and 𝐷1 and Here 𝜀v 𝐷2 are model input parameters. 𝑋0 is the initial location of the cap when 𝜅 = 𝜅0. ). The five input parameters (𝑋0, 𝑊, 𝐷1, 𝐷2, and 𝑅) are obtained from fits to the pressure-volumetric strain curves in isotropic compression and uniaxial strain. 𝑋0 determines the pressure at which compaction initiates in isotropic compression. 𝑅 combined with 𝑋0, determines the pressure at which compaction initiates in uniaxial strain. 𝐷1 and 𝐷2 determine the shape of the pressure-volumetric strain curves. 𝑊 determines the maximum plastic volume compaction. Shear Hardening Surface. In unconfined compression, the stress-strain behavior of concrete exhibits nonlinearity and dilation prior to the peak. Such behavior is be modeled with an initial shear yield surface, 𝑁H𝐹f, which hardens until it coincides with the ultimate shear yield surface, 𝐹f. Two input parameters are required. One parameter, 𝑁H, initiates hardening by setting the location of the initial yield surface. A second parameter, 𝐶H, determines the rate of hardening (amount of nonlinearity). Damage. Concrete exhibits softening in the tensile and low to moderate compressive regimes. 𝑑 = (1 − 𝑑)𝜎𝑖𝑗 𝜎𝑖𝑗 vp, (22.111.9) A scalar damage parameter, 𝑑, transforms the viscoplastic stress tensor without damage, denoted 𝜎 vp, into the stress tensor with damage, denoted 𝜎 d. Damage accumulation is based upon two distinct formulations, which we call brittle damage and ductile damage. The initial damage threshold is coincident with the shear plasticity surface, so the threshold does not have to be specified by the user. Ductile Damage. Ductile damage accumulates when the pressure (𝑃) is compressive and an energy-type term, 𝜏c, exceeds the damage threshold, 𝜏0c. Ductile damage accumulation depends upon the total strain components, 𝜀𝑖𝑗, as follows: 𝜏c = √ 𝜎𝑖𝑗𝜀𝑖𝑗 (22.111.10) The stress components 𝜎𝑖𝑗 are the elasto-plastic stresses (with kinematic hardening) calculated before application of damage and rate effects. LS-DYNA Theory Manual Material Models Brittle Damage. Brittle damage accumulates when the pressure is tensile and an energy-type term, 𝜏t, exceeds the damage threshold, 𝜏0t. Brittle damage accumulation depends upon the maximum principal strain, 𝜀max, as follows: 𝜏t = √𝐸𝜀max . (22.111.11) Softening Function. As damage accumulates, the damage parameter 𝑑 increases from an initial value of zero, towards a maximum value of one, via the following formulations: Brittle Damage: 𝑑(𝜏1) = 0.999 ( 1 + 𝐷 1 + 𝐷exp[−𝐶(𝜏𝑡 − 𝜏0𝑡)] − 1). Ductile Damage: 𝑑(𝜏1) = 𝑑max ( 1 + 𝐵 1 + 𝐵exp[−𝐴(𝜏c − 𝜏0c)] − 1). (22.111.12) (22.111.13) The damage parameter that is applied to the six stresses is equal to the current maximum of the brittle or ductile damage parameter. The parameters 𝐴 and 𝐵 or 𝐶 and 𝐷 set the shape of the softening curve plotted as stress-displacement or stress-strain. The parameter 𝑑max is the maximum damage level that can be attained. It is internally calculated and is less than one at moderate confining pressures . The compressive softening parameter, 𝐴, may also be reduced with confinement, using the input parameter PMOD, as follows: 𝐴 = 𝐴(𝑑max + 0.001)PMOD. (22.111.14) Regulating Mesh Size Sensitivity. The concrete model maintains constant fracture energy, regardless of element size. The fracture energy is defined here as the area under the stress-displacement curve from peak strength to zero strength. This is done by internally formulating the softening parameters 𝐴 and 𝐶 in terms of the element length, 𝑙 (cube root of the element volume), the fracture energy, 𝐺f, the initial damage threshold, 𝜏0t or 𝜏0c, and the softening shape parameters, 𝐷 or 𝐵. The fracture energy is calculated from up to five user-specified input parameters (𝐺fc, 𝐺ft, 𝐺fs, pwrc, pwrc). The user specifies three distinct fracture energy values. These are the fracture energy in uniaxial tensile stress, 𝐺ft, pure shear stress, 𝐺fs, and uniaxial compressive stress, 𝐺fc. The model internally selects the fracture energy from equations which interpolate between the three fracture energy values as a function of the stress state (expressed via two stress invariants). The interpolation equations depend upon the user-specified input powers PWRC and PWRT, as follows. if the pressure is tensile (22.111.15) Material Models LS-DYNA Theory Manual 𝐺f = 𝐺fs + trans(𝐺ft − 𝐺fs) where trans = if the pressure is compressive PWRT ⎜⎜⎜⎛ −𝐽1 √3𝐽′ ⎝ ⎟⎟⎟⎞ 2⎠ 𝐺f = 𝐺fs + trans(𝐺fc − 𝐺fs) where trans = PWRC ⎜⎜⎜⎛ 𝐽1 ⎟⎟⎟⎞ √3𝐽′2⎠ ⎝ The internal parameter trans is limited to range between 0 and 1. Element Erosion. An element loses all strength and stiffness as 𝑑 → 1. To prevent computational difficulties with very low stiffness, element erosion is available as a user option. An element erodes when 𝑑 > 0.99 and the maximum principal strain is greater than a user supplied input value, 1-erode. Viscoplastic Rate Effects. At each time step, the viscoplastic algorithm interpolates p, to between the elastic trial stress, 𝜎𝑖𝑗 set the viscoplastic stress (with rate effects), 𝜎𝑖𝑗 T, and the inviscid stress (without rate effects), 𝜎𝑖𝑗 vp: vp = (1 − 𝛾)𝜎𝑖𝑗 𝜎𝑖𝑗 p, T + 𝛾𝜎𝑖𝑗 (22.111.16) with 𝛾 = Δ𝑡/𝜂 1+Δ𝑡/𝜂. This interpolation depends upon the effective fluidity coefficient, , and the time step, 𝑡. The effective fluidity coefficient is internally calculated from five user-supplied input parameters and interpolation equations: if the pressure is tensile 𝜂 = 𝜂s + trans(𝜂t − 𝜂s) trans = if the pressure is compressive 𝜂 = 𝜂s + trans(𝜂c − 𝜂s) trans = 𝜂t = 𝜂0t 𝜀̇Nt 𝜂c = 𝜂0c 𝜀̇Nc 𝜂s = SRATE 𝜂t pwrt ⎜⎜⎜⎛ −𝐽1 √3𝐽′ ⎝ ⎟⎟⎟⎞ 2⎠ pwrc ⎜⎜⎜⎛ 𝐽1 √3𝐽′ ⎝ ⎟⎟⎟⎞ 2⎠ (22.111.17) The input parameters are 𝜂0t and 𝑁t for fitting uniaxial tensile stress data, 𝜂0c and 𝑁c for fitting the uniaxial compressive stress data, and SRATE for fitting shear stress data. The effective strain rate is 𝜀̇. This viscoplastic model may predict substantial rate effects at high strain rates (𝜀̇ > 100). To limit rate effects at high strain rates, the user may input overstress limits in tension (OVERT) and compression (OVERC). These input parameters limit calculation of the fluidity parameter, as follows: LS-DYNA Theory Manual Material Models If 𝐸𝜀̇𝜂 > OVER, then = over 𝛦𝜀̇ (22.111.18) where OVER = OVERT when the pressure is tensile, and OVER = OVERC when the pressure is compressive. The user has the option of increasing the fracture energy as a function of effective strain rate via the REPOW input parameter, as follows: rate = 𝐺f 𝐺f ⎜⎛1 + ⎝ 𝐸𝜀̇𝜂 ⎟⎞ 𝑟𝑠√𝐸⎠ REPOW (22.111.19) rate is the fracture energy enhanced by rate effects, and 𝑟𝑠 is the internally Here 𝐺f calculated damage threshold before application of rate effects . The term in brackets is greater than, or equal to one, and is the approximate ratio of the dynamic to static strength. Material Models LS-DYNA Theory Manual 22.112 Material Models 161 and 162: Composite MSC in The unidirectional and fabric layer failure criteria and the associated property degradation models for material 161 are described as follows. All the failure criteria are stresses expressed (𝜎𝑎, 𝜎𝑏, 𝜎𝑐, 𝜏𝑎𝑏, 𝜏𝑏𝑐, 𝜏𝑐𝑎) and the associated elastic moduli are (𝐸𝑎, 𝐸𝑏, 𝐸𝑐, 𝐺𝑎𝑏, 𝐺𝑏𝑐, 𝐺𝑐𝑎). Note that for the unidirectional model, 𝑎, 𝑏 and 𝑐 denote the fiber, in-plane transverse and out-of-plane directions, respectively, while for the fabric model, 𝑎, 𝑏 and 𝑐 denote the in-plane fill, in-plane warp and out-of-plane directions, respectively. components based on ply terms of stress level Unidirectional Lamina Model Three criteria are used for fiber failure, one in tension/shear, one in compression and another one in crush under pressure. They are chosen in terms of quadratic stress forms as follows: Tensile/shear fiber mode: 𝑓1 = ( ) 〈𝜎𝑎〉 𝑆𝑎T + ( 2 + 𝜏𝑐𝑎 𝜏𝑎𝑏 𝑆FS ) − 1 = 0. Compression fiber mode: 𝑓2 = ( ′〉 〈𝜎𝑎 𝑆𝑎C ) − 1 = 0, ′ = −𝜎𝑎 + ⟨− 𝜎𝑎 𝜎𝑏 + 𝜎𝑐 ⟩. Crush mode: 𝑓3 = ( ) 〈𝑝〉 𝑆FC − 1 = 0, 𝑝 = − 𝜎𝑎 + 𝜎𝑏 + 𝜎𝑐 . (22.112.1) (22.112.2) (22.112.3) ⟩ are Macaulay brackets, 𝑆𝑎T and 𝑆𝑎C are the tensile and compressive strengths where ⟨ in the fiber direction, and 𝑆FS and 𝑆FC are the layer strengths associated with the fiber shear and crush failure, respectively. Matrix mode failures must occur without fiber failure, and hence they will be on planes parallel to fibers. For simplicity, only two failure planes are considered: one is perpendicular to the planes of layering and the other one is parallel to them. The matrix failure criteria for the failure plane perpendicular and parallel to the layering planes, respectively, have the forms: Perpendicular matrix mode: 𝑓4 = ( ) ⟨𝜎𝑏⟩ 𝑆𝑏T + ( 𝜏𝑏𝑐 ′ ) 𝑆𝑏𝑐 + ( 𝜏𝑎𝑏 𝑆𝑎𝑏 ) − 1 = 0. Parallel matrix mode (Delamination): 22-264 (Material Models) LS-DYNA Theory Manual Material Models 2 𝑓5 = 𝑆2 {⎧ ⎩{⎨ ( ⟨𝜎𝑐⟩ 𝑆𝑏T ) + ( ) 𝜏𝑏𝑐 " 𝑆𝑏𝑐 + ( 𝜏𝑐𝑎 𝑆𝑐𝑎 ) }⎫ ⎭}⎬ − 1 = 0, (22.112.5) where 𝑆𝑏T is the transverse tensile strength. Based on the Coulomb-Mohr theory, the shear strengths for the transverse shear failure and the two axial shear failure modes are assumed to be the forms, 𝑆𝑎𝑏 = 𝑆𝑎𝑏 ′ = 𝑆𝑏𝑐 𝑆𝑏𝑐 𝑆𝑐𝑎 = 𝑆𝑐𝑎 " = 𝑆𝑏𝑐 𝑆𝑏𝑐 (0) + tan(𝜑)⟨−𝜎𝑏⟩, (0) + tan(𝜑)⟨−𝜎𝑏⟩, (0) + tan(𝜑)⟨−𝜎𝑐⟩, (0) + tan(𝜑)⟨−𝜎𝑐⟩, (22.112.6) where 𝜑 is a material constant as tan(𝜑) is similar to the coefficient of friction, and 𝑆𝑎𝑏 (0)are the shear strength values of the corresponding tensile modes. (0) and 𝑆𝑏𝑐 𝑆𝑐𝑎 (0), Failure predicted by the criterion of 𝑓4 can be referred to as transverse matrix failure, while the matrix failure predicted by 𝑓5, which is parallel to the layer, can be referred as the delamination mode when it occurs within the elements that are adjacent to the ply interface. Note that a scale factor 𝑆 is introduced to provide better correlation of delamination area with experiments. The scale factor 𝑆 can be determined by fitting the analytical prediction to experimental data for the delamination area. When fiber failure in tension/shear mode is predicted in a layer by 𝑓1, the load carrying capacity of that layer is completely eliminated. All the stress components are reduced to zero instantaneously (100 time steps to avoid numerical instability). For compressive fiber failure, the layer is assumed to carry a residual axial load, while the transverse load carrying capacity is reduced to zero. When the fiber compressive failure mode is reached due to 𝑓2, the axial layer compressive strength stress is assumed to reduce to a residual value SRC (=SFFC ∗ SAC). The axial stress is then assumed to remain constant, i.e., 𝜎𝑎 = −𝑆RC, for continuous compressive loading, while the subsequent unloading curve follows a reduced axial modulus to zero axial stress and strain state. When the fiber crush failure occurs, the material is assumed to behave elastically for compressive pressure, 𝑝 > 0, and to carry no load for tensile pressure, 𝑝 < 0. (0)and 𝑆𝑏𝑐 When a matrix failure (delamination) in the a-b plane is predicted, the strength (0) are set to zero. This results in reducing the stress components 𝜎𝑐, values for 𝑆𝑐𝑎 𝜏𝑏𝑐 and 𝜏𝑐𝑎 to the fractured material strength surface. For tensile mode, 𝜎𝑐 > 0, these stress components are reduced to zero. For compressive mode, 𝜎𝑐 < 0, the normal stress 𝜎𝑐 is assumed to deform elastically for the closed matrix crack. Loading on the failure envelop, the shear stresses are assumed to ‘slide’ on the fractured strength surface (frictional shear stresses) like in an ideal plastic material, while the subsequent unloading shear stress-strain path follows reduced shear moduli to the zero shear stress and strain state for both 𝜏𝑏𝑐 and 𝜏𝑐𝑎 components. Material Models LS-DYNA Theory Manual (0)and 𝑆𝑏𝑐 The post failure behavior for the matrix crack in the a-c plane due to 𝑓4 is modeled in the same fashion as that in the a-b plane as described above. In this case, (0)are reduced to zero instantaneously. The post fracture when failure occurs, 𝑆𝑎𝑏 (0) = 0. For tensile response is then governed by failure criterion of f5 with 𝑆𝑎𝑏 mode, 𝜎𝑏, , 𝜏𝑎𝑏 and 𝜏𝑏𝑐 are zero. For compressive mode, 𝜎𝑏 < 0, 𝜎𝑏 is assumed to be elastic, while 𝜏𝑎𝑏 and 𝜏𝑏𝑐 ‘slide’ on the fracture strength surface as in an ideal plastic material, and the unloading path follows reduced shear moduli to the zero shear stress and strain state. It should be noted that 𝜏𝑏𝑐 is governed by both the failure functions and should lie within or on each of these two strength surfaces. (0) = 0 and 𝑆𝑏𝑐 Fabric Lamina Model The fiber failure criteria of Hashin for a unidirectional layer are generalized to characterize the fiber damage in terms of strain components for a plain weave layer. The fill and warp fiber tensile/shear failure are given by the quadratic interaction between the associated axial and shear stresses, i.e. 𝑓6 = ( ) ⟨𝜎𝑎⟩ 𝑆𝑎T + (𝜏𝑎𝑏 2 + 𝜏𝑐𝑎 2 ) 𝑆𝑎FS − 1 = 0, 𝑓7 = ( ⟨𝜎𝑏⟩ 𝑆𝑏T ) + (𝜏𝑎𝑏 2 ) 2 + 𝜏𝑏𝑐 𝑆𝑏FS − 1 = 0, (22.112.7) (22.112.8) where 𝑆𝑎T and 𝑆𝑏T are the axial tensile strengths in the fill and warp directions, respectively, and 𝑆𝑎FS and 𝑆𝑏FS are the layer shear strengths due to fiber shear failure in the fill and warp directions. These failure criteria are applicable when the associated 𝜎𝑎 or 𝜎𝑏 is positive. It is assumed 𝑆aFS = SFS, and 𝑆𝑏T 𝑆𝑎T 𝑆𝑏FS = SFS ∗ (22.112.9) . When 𝜎𝑎 or 𝜎𝑏is compressive, it is assumed that the in-plane compressive failure in both the fill and warp directions are given by the maximum stress criterion, i.e. 𝑓8 = [ ] ′⟩ ⟨𝜎𝑎 𝑆𝑎C 𝑓9 = [ ] ′⟩ ⟨𝜎𝑏 𝑆𝑏C − 1 = 0, ′ = −𝜎𝑎 + ⟨−𝜎𝑐⟩, 𝜎𝑎 (22.112.10) − 1 = 0, ′ = −𝜎𝑏 + ⟨−𝜎𝑐⟩. 𝜎𝑏 (22.112.11) where 𝑆𝑎C and 𝑆𝑏C are the axial compressive strengths in the fill and warp directions, respectively. The crush failure under compressive pressure is 𝑓10 = ( ⟨𝑝⟩ 𝑆FC ) − 1 = 0, 𝑝 = − 𝜎𝑎 + 𝜎𝑏 + 𝜎𝑐 . (22.112.12) LS-DYNA Theory Manual Material Models A plain weave layer can fail under in-plane shear stress without the occurrence of fiber breakage. This in-plane matrix failure mode is given by 𝑓11 = ( 𝜏𝑎𝑏 𝑆𝑎𝑏 ) − 1 = 0, (22.112.13) where 𝑆𝑎𝑏 is the layer shear strength due to matrix shear failure. Another failure mode, which is due to the quadratic interaction between the thickness stresses, is expected to be mainly a matrix failure. This through the thickness matrix failure criterion is 𝑓12 = 𝑆2 {( ) ⟨𝜎𝑐⟩ 𝑆𝑐𝑇 + ( 𝜏𝑏𝑐 𝑆𝑏𝑐 ) + ( 𝜏𝑐𝑎 𝑆𝑐𝑎 ) } − 1 = 0, (22.112.14) where 𝑆𝑐T is the through the thickness tensile strength, and 𝑆𝑏𝑐, and 𝑆𝑐𝑎 are the shear strengths assumed to depend on the compressive normal stress sc, i.e., { 𝑆𝑐𝑎 𝑆𝑏𝑐 } = { (0) 𝑆𝑐𝑎 (0)} + tan(𝜑)⟨−𝜎𝑐⟩. 𝑆𝑏𝑐 (22.112.15) When failure predicted by this criterion occurs within elements that are adjacent to the ply interface, the failure plane is expected to be parallel to the layering planes, and, thus, can be referred to as the delamination mode. Note that a scale factor 𝑆 is introduced to provide better correlation of delamination area with experiments. The scale factor 𝑆 can be determined by fitting the analytical prediction to experimental data for the delamination area. Similar to the unidirectional model, when fiber tensile/shear failure is predicted in a layer by 𝑓6 or 𝑓7, the load carrying capacity of that layer in the associated direction is completely eliminated. For compressive fiber failure due to 𝑓8 or 𝑓9, the layer is assumed to carry a residual axial load in the failed direction, while the load carrying capacity transverse to the failed direction is assumed unchanged. When the compressive axial stress in a layer reaches the compressive axial strength 𝑆𝑎C or 𝑆𝑏C, the axial layer stress is assumed to be reduced to the residual strength 𝑆aRC or 𝑆bRC where 𝑆aRC = SFFC ∗ SaC and SbRC = SFFC ∗ SbC. The axial stress is assumed to remain constant, i.e., 𝜎𝑎 = −𝑆aCR or 𝜎𝑏 = −SbCR, for continuous compressive loading, while the subsequent unloading curve follows a reduced axial modulus. When the fiber crush failure has occurred, the material is assumed to behave elastically for compressive pressure, 𝑝 > 0, and to carry no load for tensile pressure, 𝑝 < 0. When the in-plane matrix shear failure is predicted by f11 the axial load carrying capacity within a failed element is assumed unchanged, while the in-plane shear stress is assumed to be reduced to zero. Material Models LS-DYNA Theory Manual For through the thickness matrix (delamination) failure given by equations 𝑓12, the in-plane load carrying capacity within the element is assumed to be elastic, while (0), are set to zero. For tensile mode, the strength values for the tensile mode, 𝑆𝑐𝑎 𝜎𝑐 > 0, the through the thickness stress components are reduced to zero. For compressive mode, 𝜎𝑐 < 0, 𝜎𝑐 is assumed to be elastic, while 𝜏𝑏𝑐 and 𝜏𝑐𝑎 ‘slide’ on the fracture strength surface as in an ideal plastic material, and the unloading path follows reduced shear moduli to the zero shear stress and strain state. (0)and 𝑆𝑏𝑐 The effect of strain-rate on the layer strength values of the fiber failure modes is modeled by the strain-rate dependent functions for the strength values {IRT} as {SRT } = {S0 } ( 1 + Crate1 ln ̇} {ε̅ ), ε̇0 {𝑆RT } = ⎧𝑆𝑎T ⎫ } { } { 𝑆𝑎C } { } { 𝑆𝑏T ⎬ ⎨ 𝑆𝑏C } { } { 𝑆FC } { } { 𝑆FS ⎭ ⎩ and {𝜀̅ ̇} = ⎧ { { { { { ⎨ { { { { { ⎩ ∣𝜀̇𝑎∣ ⎫ } } ∣𝜀̇𝑎∣ } } ∣𝜀̇𝑏∣ } ∣𝜀̇𝑏∣ ⎬ } ∣𝜀̇𝑐∣ } } } } 2 ) 2 + 𝜀̇𝑏𝑐 2⎭ (𝜀̇𝑐𝑎 , (22.112.16) (22.112.17) where 𝐶rate is the strain-rate constants, and {𝑆0 }are the strength values of {𝑆RT } at the reference strain-rate 𝜀̇0. Damage Model The damage model is a generalization of the layer failure model of Material 161 by adopting the MLT damage mechanics approach, Matzenmiller et al. [1995], for characterizing the softening behavior after damage initiation. Complete model description is given in Yen [2001]. The damage functions, which are expressed in terms of ply level engineering strains, are converted from the above failure criteria of fiber and matrix failure modes by neglecting the Poisson’s effect. Elastic moduli reduction is expressed in terms of the associated damage parameters 𝜛𝑖: ′ = (1 − ϖ𝑖)E𝑖 E𝑖 (22.112.18) 𝑚𝑖/𝑚𝑖) 𝑟𝑖 ≥ 0 𝑖 = 1, . . . ,6, ϖ𝑖 = 1 − exp(−𝑟𝑖 (22.112.19) ′ are the reduced elastic moduli, 𝑟𝑖 are the where 𝐸𝑖 are the initial elastic moduli, 𝐸𝑖 damage thresholds computed from the associated damage functions for fiber damage, matrix damage and delamination, and mi are material damage parameters, which are currently assumed to be independent of strain-rate. The damage function is formulated to account for the overall nonlinear elastic response of a lamina including the initial ‘hardening’ and the subsequent softening beyond the ultimate strengths. In the damage model (Material 162), the effect of strain-rate on the nonlinear stress-strain response of a composite layer is modeled by the strain-rate dependent functions for the elastic moduli {𝐸RT } as LS-DYNA Theory Manual Material Models {𝐸RT } = {𝐸0 } ( 1 + {𝐶rate} ln ̇} {𝜀̅ ), 𝜀̇0 {𝐸RT } = ⎧ 𝐸𝑎 ⎫ }} {{ 𝐸𝑏 }} {{ 𝐸𝑐 ⎬ ⎨ 𝐺𝑎𝑏 }} {{ 𝐺𝑏𝑐 }} {{ 𝐺𝑐𝑎⎭ ⎩ , {𝜀̅ ̇} = ⎧ ∣𝜀̇𝑎∣ ⎫ } { } { ∣𝜀̇𝑏∣ } { } { ∣𝜀̇𝑐∣ ⎬ ⎨ ∣𝜀̇𝑎𝑏∣ } { } { ∣𝜀̇𝑏𝑐∣ } { } { ∣𝜀̇𝑐𝑎∣⎭ ⎩ and {𝐶rate} = ⎧𝐶rate2 ⎫ } { } { 𝐶rate2 } { } { 𝐶rate4 ⎬ ⎨ 𝐶rate3 } { } { 𝐶rate3 } { } { 𝐶rate3⎭ ⎩ , (22.112.20) (22.112.21) where {𝐶rate} are the strain-rate constants. {𝐸0} are the modulus values of {𝐸RT } at the reference strain-rate 𝜀̇0. Material Models LS-DYNA Theory Manual 22.113 Material Model 163: Modified Crushable Foam The volumetric strain is defined in terms of the relative volume, 𝑉, as: 𝛾 = 1. −𝑉. The relative volume is defined as the ratio of the current to the initial volume. In place of the effective plastic strain in the D3PLOT database, the integrated volumetric strain is output. This material is an extension of material 63, *MAT_CRUSHABLE_FOAM. It allows the yield stress to be a function of both volumetric strain rate and volumetric strain. Rate effects are accounted for by defining a table of curves using *DEFINE_TABLE. Each curve defines the yield stress versus volumetric strain for a different strain rate. The yield stress is obtained by interpolating between the two curves that bound the strain rate. To prevent high frequency oscillations in the strain rate from causing similar high frequency oscillations in the yield stress, a modified volumetric strain rate is used when interpolating to obtain the yield stress. The modified strain rate is obtained as follows. If NCYCLE is > 1, then the modified strain rate is obtained by a time average of the actual strain rate over NCYCLE solution cycles. For SRCLMT > 0, the modified strain rate is capped so that during each cycle, the modified strain rate is not permitted to change more than SRCLMT multiplied by the solution time step. Figure 22.113.1. Rate effects are defined by a family of curves giving yield stress versus volumetric strain. 1-V LS-DYNA Theory Manual Material Models 22.114 Material Model 164: Brain Linear Viscoelastic The shear relaxation behavior is described by the Maxwell model as: 𝐺(𝑡) = 𝐺 + (𝐺0 − 𝐺∞)𝑒−𝛽𝑡. (22.114.1) A Jaumann rate formulation is used 𝛻 𝜎′𝑖𝑗 = 2 ∫ 𝐺(𝑡 − 𝜏) 𝐷′𝑖𝑗(𝜏)𝑑𝑡 . (22.114.2) 𝛻 where the prime denotes the deviatoric part of the stress rate, 𝜎 . For the Kelvin model the stress evolution equation is defined as: 𝑖𝑗, and the strain rate 𝐷𝑖𝑗 𝑠 ̇𝑖𝑗 + 𝑠𝑖𝑗 = (1 + 𝛿𝑖𝑗) (𝐺0 + 𝐺∞ ) 𝑒 ̇𝑖𝑗. (22.114.3) The strain data as written to the LS-DYNA database may be used to predict damage, see [Bandak 1991]. Material Models LS-DYNA Theory Manual 22.115 Material Model 166: Moment Curvature Beam Curvature rate can be decomposed into elastic part and plastic part: 𝜀̇ = 𝜀̇e + 𝜀̇p ⇒ 𝜀̇ = 𝜀̇p + 𝜀̇p ⇒ 𝜅̇ = 𝜅̇e + 𝜅p. (22.115.1) Moment rate is the product of elastic bending stiffness and elastic curvature: 𝑀̇ = ∫ 𝜎̇ 𝑦𝑑𝐴 = ∫ 𝐸e𝜀̇e𝑦𝑑𝐴 = ∫ 𝐸e𝜅̇e𝑦2𝑑𝐴 = ∫ 𝐸e(𝜅̇ − 𝜅̇p)𝑦2𝑑𝐴 = 𝐸e(𝜅̇ − 𝜅̇p) ∫ 𝑦2𝑑𝐴 = (𝐸𝐼)e(𝜅̇ − 𝜅̇p) . Plastic flow rule: 𝜓 = |𝑀| (Isotropic hardening) (22.115.2) 𝜅̇p = 𝜆̇ 𝜕𝜓 𝜕𝑀 Yield condition: = 𝜆̇sign(𝑀), 𝜅̅ ̇p = √𝜅̇p𝜅̇p = 𝜆̇. (22.115.3) 𝑓 = |𝑀| − 𝑀Y(𝜅̅p) = 0. Loading and unloading conditions: 𝜆̇ ≥ 0, 𝑓 ≤ 0, 𝜆̇𝑓 = 0. Consistency condition: 𝑓 ̇ = 0 ⇒ 𝑀̇ sign(𝑀) − ̇p ⇒ 𝜆̇ ≡ 𝜅̅ 𝑀sign(𝑀) (𝐸𝐼)p = = ∂𝑀Y ∂𝜅̅p 𝜅̅p = 0 (𝐸𝐼)e (𝐸𝐼)p (𝜅̇ − 𝜅̇p) sign(𝑀) = (𝐸𝐼)e (𝐸𝐼)p [𝜅̇ − 𝜆̇ sign(𝑀)]sign(𝑀) ̇ = (𝐸𝐼)e𝜅̇ sign(𝑀) (𝐸𝐼)p + (𝐸𝐼)e ⇒ 𝜆̇ ≡ 𝜅̅ (22.115.4) (22.115.5) (22.115.6) Moment rate is also the product of tangential bending stiffness and total curvature: 𝑀̇ = (𝐸𝐼)ep𝜅̇. (22.115.7) Elastic, plastic, and tangential stiffnesses are obtained from user-defined curves: (𝐸𝐼)ep = 𝑑𝑀 𝑑𝜅 , (𝐸𝐼)p = 𝑑𝑀 𝑑𝜅̅p. (22.115.8) Both are obtained from user-defined curves. LS-DYNA Theory Manual Material Models (𝐸𝐼)ep(𝐸𝐼)p (𝐸𝐼)p − (𝐸𝐼)ep. For Torsion-Twist, simply replace 𝑀 by 𝑇, 𝜅 by 𝛽, (𝐸𝐼) by (𝐺𝐽). For Force-Strain, simply replace 𝑀 by 𝑁, 𝜅 by 𝜀, (𝐸𝐼) by (𝐸𝐴). (𝐸𝐼)e = (22.115.9) Material Models LS-DYNA Theory Manual 22.116 Material Model 169: Arup Adhesive The through-thickness direction is identified from the smallest dimension of each element. It is expected that this dimension will be much smaller than in-plane dimensions (typically 2mm compared with 10mm). In-plane stresses are set to zero: it is assumed that the stiffness and strength of the substrate is large compared with that of the adhesive, given the relative thicknesses. If the substrate is modeled with shell elements, it is expected that these will lie at the mid-surface of the substrate geometry. Therefore the solid elements representing the adhesive will be thicker than the actual bond. The yield and failure surfaces are treated as a power-law combination of direct tension and shear across the bond: (𝜎/ 𝜎max)PWRT + (𝜏/𝜏max)PWRS = 1.0 at yield. The stress-displacement curves for tension and shear are shown in the diagrams below. In both cases, 𝐺c is the area under the curve. Because of the algorithm used, yielding in tension across the bond does not require strains in the plane of the bond – unlike the plasticity models, plastic flow is not treated as volume-conserving. The Plastic Strain output variable has a special meaning: • 0 < ps < 1: ps is the maximum value of the yield function experienced since time zero • 1 < ps < 2: the element has yielded and the strength is reducing towards failure – yields at ps = 1, fails at ps = 2. Stress Stress TENMAX SHRMAX Area = Gcten Failure dp = SHRP.dfs Area = Gcshr Failure dft Displacement Tension dp Shear dfs Displacement Figure 22.116.1. LS-DYNA Theory Manual Material Models 22.117 Material Model 170: Resultant Anisotropic The in-plane elastic matrix for in-plane plane stress behavior is given by: 𝐂in plane = 𝑄11p 𝑄12p ⎡ 𝑄12p 𝑄22p ⎢ ⎢ ⎢ ⎢ ⎢ ⎣ 𝑄44p 𝑄55p ⎤ ⎥ ⎥ . ⎥ ⎥ ⎥ 𝑄66p⎦ The terms Q𝑖𝑗p are defined as: 𝑄11p = 𝑄22p = 𝑄12p = 𝐸11p 1 − 𝜈12p𝜈21p 𝐸22p 1 − 𝜈12p𝜈21p 𝜈12p𝐸11p 1 − 𝜈12p𝜈21p , , , 𝑄44p = 𝐺12p, 𝑄55p = 𝐺23p, 𝑄66p = 𝐺31p. The elastic matrix for bending behavior is given by: 𝐂bending = 𝑄11b 𝑄12b 𝑄12b 𝑄22b ⎡ ⎢ ⎣ ⎤. ⎥ 𝑄44b⎦ The terms 𝑄𝑖𝑗b are similarly defined. (22.117.1) (22.117.2) (22.117.3) Material Models LS-DYNA Theory Manual 22.118 Material Model 175: Viscoelastic Maxwell Rate effects are taken into accounted through linear viscoelasticity by a convolution integral of the form: 𝜎𝑖𝑗 = ∫ 𝑔𝑖𝑗𝑘𝑙(𝑡 − 𝜏) 𝜕𝜀𝑘𝑙 𝜕𝜏 𝑑𝜏 , (22.118.1) where 𝑔𝑖𝑗𝑘𝑙(𝑡 − 𝜏) is the relaxation function for different stress measures. This stress is added to the stress tensor determined from the strain energy functional. If we wish to include only simple rate effects, the relaxation function is represented by six terms from the Prony series: 𝑔(𝑡) = ∑ 𝐺𝑚𝑒−𝛽𝑚𝑡 𝑚=1 . (22.118.2) We characterize this in the input by shear moduli, 𝐺𝑖, and the decay constants, 𝛽𝑖. An arbitrary number of terms, up to 6, may be used when applying the viscoelastic model. For volumetric relaxation, the relaxation function is also represented by the Prony series in terms of bulk moduli: 𝑘(𝑡) = ∑ 𝐾𝑚𝑒−𝛽𝑘𝑚𝑡 . 𝑚=1 (22.118.3) The Arrhenius and Williams-Landau-Ferry (WLF) shift functions account for the effects of the temperature on the stress relaxation. A scaled time, 𝑡′, 𝑡′ = ∫ 𝛷(𝑇)𝑑𝑡 , (22.118.4) is used in the relaxation function instead of the physical time. The Arrhenius shift function is 𝛷(𝑇) = exp (−𝐴 { − 𝑇REF }), and the Williams-Landau-Ferry shift function is 𝛷(𝑇) = exp (−𝐴 𝑇 − TREF 𝐵 + 𝑇 − 𝑇REF ). (22.118.5) (22.118.6) LS-DYNA Theory Manual Material Models 22.119 Material Model 176: Quasilinear Viscoelastic The equations for this model are given as: 𝜎(𝑡) = ∫ 𝐺(𝑡 − 𝜏) 𝜕𝜎𝜀[𝜀(𝜏)] 𝜕𝜀 𝜕𝜀 𝜕𝜏 𝑑𝜏, 𝐺(𝑡) = ∑ 𝐺𝑖 𝑖=1 𝜎𝜀(𝜀) = ∑ 𝐶𝑖 𝑖=1 𝑒−𝛽𝑡, 𝜀𝑖, (22.119.1) where G is the shear modulus. In place of the effective plastic strain in the D3PLOT database, the effective strain is output: 𝜀effective = √ 𝜀𝑖𝑗𝜀𝑖𝑗. (22.119.2) The polynomial for instantaneous elastic response should contain only odd terms if symmetric tension-compression response is desired. Material Models LS-DYNA Theory Manual 22.120 Material Models 177 and 178: Hill Foam and Viscoelastic Hill Foam 22.120.1 Hyperelasticity Using the Principal Stretch Ratios Material types 177 and 178 in LS-DYNA are highly compressible Ogden models combined with viscous stress contributions. The latter model also allows for an additive viscoelastic stress contribution. As for the rate independent part, the constitutive law is determined by a strain energy function that is expressed in terms of the principal stretches, i.e., 𝑊 = 𝑊(𝜆1, 𝜆2, 𝜆3). To obtain the Cauchy stress 𝜎𝑖𝑗, as well as TC, they are first calculated in the principal basis the constitutive tensor of interest, 𝐶𝑖𝑗𝑘𝑙 after which they are transformed back to the “base frame”, or standard basis. The complete set of formulas is given by Crisfield [1997] and is for the sake of completeness recapitulated here. The principal Kirchhoff stress components are given by E = 𝜆𝑖 𝜏𝑖𝑖 𝜕𝑊 𝜕𝜆𝑖 (no sum), that are transformed to the standard basis using the standard formula E. 𝜏𝑖𝑗 = 𝑞𝑖𝑘𝑞𝑗𝑙𝜏𝑘𝑙 (22.120.1) (22.120.2) The 𝑞𝑖𝑗 are the components of the orthogonal tensor containing the eigenvectors of the principal basis. The Cauchy stress is then given by 𝜎𝑖𝑗 = 𝐽−1𝜏𝑖𝑗, (22.120.3) where 𝐽 = 𝜆1𝜆2𝜆3 is the relative volume change. The constitutive tensor that relates the rate of deformation to the Truesdell (convected) rate of Kirchhoff stress in the principal basis can be expressed as TKE = 𝜆𝑗 𝐶𝑖𝑖𝑗𝑗 TKE = 𝐶𝑖𝑗𝑖𝑗 TKE = 𝐶𝑖𝑗𝑖𝑗 E𝛿𝑖𝑗 − 2𝜏𝑖𝑖 𝜕𝜏𝑖𝑖 𝜕𝜆𝑗 2𝜏𝑗𝑗 E − 𝜆𝑖 2𝜏𝑖𝑖 𝜆𝑗 2 − 𝜆𝑗 𝜆𝑖 𝜕𝜏𝑖𝑖 ( 𝜕𝜆𝑖 𝜆𝑖 − 𝜕𝜏𝑖𝑖 𝜕𝜆𝑗 , 𝑖 ≠ 𝑗, 𝜆𝑖 ≠ 𝜆𝑗 ), 𝑖 ≠ 𝑗, 𝜆𝑖 = 𝜆𝑗 ⎫ } } } } } } ⎬ } } } } } } ⎭ (no sum). (22.120.4) These components are transformed to the standard basis according to LS-DYNA Theory Manual Material Models TK = 𝑞𝑖𝑝𝑞𝑗𝑞𝑞𝑘𝑟𝑞𝑙𝑠𝐶𝑝𝑞𝑟𝑠 TKE, 𝐶𝑖𝑗𝑘𝑙 (22.120.5) and finally the constitutive tensor relating the rate of deformation to the Truesdell rate of Cauchy stress is obtained through TC = 𝐽−1𝐶𝑖𝑗𝑘𝑙 TK. 𝐶𝑖𝑗𝑘𝑙 (22.120.6) 22.120.2 Hill’s Strain Energy Function The strain energy function for materials 177 and 178 is given by 𝑊 = ∑ 𝑚=1 𝜇𝑚 𝛼𝑚 [𝜆1 𝛼𝑚 + 𝜆2 𝛼𝑚 + 𝜆3 𝛼𝑚 − 3 + (𝐽−𝑛𝛼𝑚 − 1)] . (22.120.7) where 𝑛, 𝜇𝑚 and 𝛼𝑚 are material parameters. To apply the formulas in the previous section, we require E = 𝜆𝑖 𝜏𝑖𝑖 𝜕𝑊 𝜕𝜆𝑖 = ∑ 𝑚=1 𝜇𝑚 𝛼𝑚 − 𝐽−𝑛𝛼𝑚). (𝜆𝑖 Proceeding with the constitutive tensor, we have 𝜆𝑗 𝜕𝜏𝑖𝑖 𝜕𝜆𝑗 = ∑ 𝜇𝑚𝛼𝑚(𝜆𝑖 𝛼𝑚𝛿𝑖𝑗 + 𝑛𝐽−𝑛𝛼𝑚) . 𝑚=1 (22.120.8) (22.120.9) In addition to the hyperelastic stress described above, a viscous stress is added. Converting to Voigt notation, this stress can be written, 𝛔 = 𝐂𝐃, (22.120.10) where 𝛔 denotes Cauchy stress, 𝐃 is the rate-of-deformation and 𝐂 is an isotropic constitutive matrix representing the viscosity. In element m, the constitutive matrix depends on the element deformation according to 𝐂 = 𝑑𝑚 𝐂𝟎, (22.120.11) where 𝑑𝑚 is the diameter4 of element m and 𝐂𝟎 is a constitutive matrix that depends only on the material parameters. The stress contribution to the internal force can be written 𝑓 int = ∫ 𝐁T𝛔𝑑𝛺𝑚, 𝛺𝑚 (22.120.12) and the corresponding material time derivative is 4 Experiments indicate that d(cid:2923) is the smallest dimension of the element. Material Models LS-DYNA Theory Manual 𝑓 ̇mat = ∫ 𝐁T𝛔∇𝑇𝑑𝛺𝑚 . 𝛺𝑚 (22.120.13) Here 𝛺𝑚 is the current configuration of element m, 𝐁 is the strain-displacement matrix and ∇𝑇 denotes the Truesdell rate of Cauchy stress. The aim is to identify the material tangent modulus through 𝑓 ̇mat = ∫ 𝐁T𝐂mat𝐁𝑑𝛺𝑚 𝑢̇, 𝛺𝑚 (22.120.14) for the viscous stress with u̇ being the nodal velocity. The Truesdell rate of the viscous stress can be written, 𝛔𝛁𝐓 = 𝐂̇𝐃 + 𝐂𝐃̇ + tr(𝐃)𝛔 − 𝐋𝛔 − 𝛔𝐋𝐓, (22.120.15) where Lis the velocity gradient. The terms on the right hand side can be treated as follows. For the first term, we can assume that 𝑑𝑚 ∝ J1/3 and then approximate 𝐂̇ = − tr(𝐃)𝐂. (22.120.16) Using Equation (22.120.10), Equation (22.120.13), the first term on the right hand side of Equation (22.120.15), Equation (22.120.16) and the expression 𝐃 = 𝐁𝐮̇, (22.120.17) a material tangent modulus contribution can be identified in Equation (22.120.14) as − 𝛔𝛅T, (22.120.18) where 𝛅 denotes the identity matrix in Voigt notation. For the second term in Equation (22.120.15), we differentiate Equation (22.120.17) to see that 𝐃̇ = 𝐁̇𝐮̇ + 𝐁𝐮̈. (22.120.19) Post-poning the treatment of the first term, the second of these two terms can be treated easily as this gives the following contribution to the material time derivative ∫ 𝐁T𝐂𝐁𝑑𝛺𝑚𝑢̇ 𝛺𝑚 𝛽Δ𝑡 , (22.120.20) where γ and 𝛽 are parameters in the Newmark scheme and Δ𝑡 is the time step. From this expression, a material tangent modulus can through Equation (22.120.14) be identified as, LS-DYNA Theory Manual Material Models 𝐂mat = 𝛽Δ𝑡 𝐂. (22.120.21) The third term in Equation (22.120.15) contributes to the material tangent modulus as resulting in a material tangent modulus given so far by 𝛔𝛅T 𝛽Δ𝑡 𝐂 + 𝛔𝛅T. 22.120.3 Viscous Stress (22.120.22) (22.120.23) From the remaining terms, i.e., the last two terms in Equation (22.120.15) and the first term in Equation (22.120.19), we see it impossible to identify contributions to a material tangent modulus. We believe that these terms must be treated in some other manner. We are thus left with two choices, either to approximate these terms within the existing framework or to attempt a thorough implementation of the correct tangent stiffness using a different, and probably demanding, approach. We reason as follows. Since this stress contribution is viscous and proportional to the mesh size, it is our belief that it serves as a stabilizing stress in the occurrence of a coarse mesh and/or large deformation rates, and really has little or nothing to do with the actual material models. If only the simulation process is slow (which it often is in an implicit analysis) and/or the mesh is sufficiently fine, this stress should be negligible compared to the other stress(es). With this in mind, we feel that it is not crucial to derive an exact tangent for this stress but we can be satisfied with an approximation. Even if attempting a more thorough derivation of the tangent stiffness, we would most certainly have to make approximations along the way. Hence we do not see this as an attractive approach. In the implementation we have simply neglected all terms involving stresses since the experience from earlier work is that such terms generally have a negative effect on the tangent if they are not absolutely correct. In addition, most of the terms involving stresses contribute to a nonsymmetric tangent stiffness, which cannot be supported by LS-DYNA at the moment. Hence the material tangent modulus for the viscous stress is given by Equation (22.120.21). We are aware of that this may be a crude approximation, and if experiments show that it is a poor one, we will take a closer look at it. In material type 178, the viscous stress acts only in the direction of the principal stretches and in compression. With C being an isotropic tensor, we evaluate the tangent stiffness modulus in the principal basis according to Equation (22.120.21), modify it to Material Models LS-DYNA Theory Manual account for the mentioned conditions and then transform it back to the global frame of reference. 22.120.4 Viscoelastic Stress Contribution For material 178, an optional viscoelastic stress contribution can be added. The evolution of this stress in time can be stated as where 12 ∇ = ∑ 2𝐺𝑚𝑠𝑖𝑗 𝜎𝑖𝑗 𝑚=1 m∇ , m, m∇ = 𝐷𝑖𝑗 − 𝛽𝑚𝑠𝑖𝑗 𝑠𝑖𝑗 (22.120.24) (22.120.25) Here 𝐺𝑚 and 𝛽𝑚 are material constants, and 𝐷𝑖𝑗 is the rate-of-deformation tensor. Referring to Borrvall [2002], we state that the tangent stiffness modulus for this stress contribution can be written 12 𝐶𝑖𝑗𝑘𝑙 = ∑ 𝐺𝑚 (𝛿𝑖𝑘𝛿𝑗𝑙 + 𝛿𝑖𝑙𝛿𝑗𝑘). 𝑚=1 (22.120.26) Just as for the viscous stress, this stress acts only in the direction of the principal stretches. Hence the tangent modulus is formed in the principal basis, modified to account for this condition and then transformed back to the global frame of reference. 22.120.5 Material Tangent Modulus for the Fully Integrated Brick To avoid locking tendencies for the fully integrated brick element in LS-DYNA, the stress is modified as 𝛔S/R = 𝛔 + (𝑝 − 𝑝̅)𝐈, (22.120.27) where 𝑝 is the pressure and 𝑝̅ is the mean pressure in the element. This affects the tangent stiffness since one has to take into account that the pressure is constant in the element. Deriving the material time derivative of the internal force results in 𝑓 ̇mat = ∫ 𝐁T𝐂𝐁𝑑𝛺𝑚 𝑢̇ + ∫ (𝑝 − 𝑝̅)𝐁T(𝐈 ⊗ 𝐈)𝐁𝑑𝛺𝑚 𝑢̇ 𝛺𝑚 𝛺𝑚 −2 ∫ (𝑝 − 𝑝̅)𝐁T𝐁𝑑𝛺𝑚 𝛺𝑚 𝑢̇ + ∫ (ṗ − p̅̅̅̅̇)BTdΩm . Ωm (22.120.28) To implement this tangent, the last term is the most difficult to deal with as it involves the time derivative (or variation) of the pressure. For certain types of material models, for instance material type 77 in LS-DYNA, the pressure is a function of the relative volume 22-282 (Material Models) 𝑝 = 𝑝(𝐽), LS-DYNA Theory Manual Material Models and with the approximation 𝑝̅ = 𝑝(𝐽 ̅), the last term can be evaluated to ∫ 𝐽𝑝′(𝐽)𝐁T(𝐈 ⊗ 𝐈)𝐁𝑑𝛺𝑚𝑢̇ 𝛺𝑚 − ∫ 𝐽 ̅𝑝′(𝐽 ̅)𝐁̅̅̅̅̅T(𝐈 ⊗ 𝐈)𝐁̅̅̅̅̅𝑑𝛺𝑚𝑢̇ , 𝛺𝑚 (22.120.30) (22.120.31) and a symmetric tangent stiffness can quite easily be implemented. We have here used 𝐽 ̅ and 𝐁̅̅̅̅̅ for the mean values of 𝐽 and 𝐁, respectively. For other types of material models, such as the ones described in this document or material type 27 in LS-DYNA, the expression for the pressure is more complicated. A characterizing feature is that a non- zero pressure can occur under constant volume. This will in general complicate the implementation of the last term and will also contribute to a non-symmetric tangent stiffness that cannot be handled in LS-DYNA at the moment. For material 27, neglecting this had a tremendous impact on the performance of the implicit solution procedure, . For the current material models, it seems to be of less importance, and we believe that this is due to the higher compressibility allowed. 22.120.6 Viscous damping Viscous damping in the model follows an implementation identical to that of material type 57. Material Models LS-DYNA Theory Manual 22.121 Material Models 179 and 180: Low Density Synthetic Foam Material types 179 and 180 in LS-DYNA are highly compressible synthetic foam models with no Poisson’s ratio effects combined with an optional visco-elastic and a stabilizing viscous stress contribution. The tensile behavior of the materials is linear where the stress cannot exceed a user prescribed cutoff stress. In compression the materials show a hysteresis on unloading similar to material 57. In addition, the first load cycle damages the material so that the stress level on reloading is significantly reduced. For material 179 the damage is isotropic while it is orthotropic for material 180. Viscous damping in the model follows an implementation identical to that of material type 57. 22.121.1 Hyperelasticity Using the Principal Stretch Ratios As for the rate independent part of the stress, the constitutive law is mainly determined by a strain energy function that is expressed in terms of the principal stretches, i.e., 𝑊 = 𝑊(𝜆1, 𝜆2, 𝜆3). To obtain the Cauchy stress 𝜎𝑖𝑗, as well as the TC, they are first calculated in the principal basis after constitutive tensor of interest, 𝐶𝑖𝑗𝑘𝑙 which they are transformed back to the “base frame”, or standard basis. The complete set of formulas is given by Crisfield [1997] and is for the sake of completeness recapitulated here. The principal Kirchhoff stress components are given by E = 𝜆𝑖 𝜏𝑖𝑖 𝜕𝑊 𝜕𝜆𝑖 (no sum), that are transformed to the standard basis using the standard formula E. 𝜏𝑖𝑗 = 𝑞𝑖𝑘𝑞𝑗𝑙𝜏𝑘𝑙 (22.121.1) (22.121.2) The 𝑞𝑖𝑗 are the components of the orthogonal tensor containing the eigenvectors of the principal basis. The Cauchy stress is then given by , 𝜎𝑖𝑗 = 𝐽−1𝜏𝑖𝑗, (22.121.3) where 𝐽 = 𝜆1𝜆2𝜆3 is the relative volume change. The constitutive tensor that relates the rate of deformation to the Truesdell (convected) rate of Kirchhoff stress can in the principal basis be expressed as LS-DYNA Theory Manual Material Models TKE = 𝜆𝑗 𝐶𝑖𝑖𝑗𝑗 TKE = 𝐶𝑖𝑗𝑖𝑗 TKE = 𝐶𝑖𝑗𝑖𝑗 E𝛿𝑖𝑗 − 2𝜏𝑖𝑖 𝜕τii 𝜕𝜆𝑗 2𝜏𝑗𝑗 E − 𝜆𝑖 2𝜏𝑖𝑖 𝜆𝑗 2 − 𝜆𝑗 𝜆𝑖 𝜕𝜏𝑖𝑖 ( 𝜕𝜆𝑖 𝜆𝑖 − 𝜕𝜏𝑖𝑖 𝜕𝜆𝑗 ), 𝑖 ≠ 𝑗, 𝜆𝑖 = 𝜆𝑗 , 𝑖 ≠ 𝑗, 𝜆𝑖 ≠ 𝜆𝑗 (no sum). (22.121.4) These components are transformed to the standard basis according to TK = 𝑞𝑖𝑝𝑞𝑗𝑞𝑞𝑘𝑟𝑞𝑙𝑠𝐶𝑝𝑞𝑟𝑠 TKE, 𝐶𝑖𝑗𝑘𝑙 (22.121.5) and finally the constitutive tensor relating the rate of deformation to the Truesdell rate of Cauchy stress is obtained through. TC = 𝐽−1𝐶𝑖𝑗𝑘𝑙 TK . 𝐶𝑖𝑗𝑘𝑙 (22.121.6) 22.121.2 Strain Energy Function The strain energy function for materials 179 and 180 is given by , W = ∑ 𝑤(λm) m=1 (22.121.7) where 𝑤(𝜆) = 2𝐸 (𝜆 − 1)2 ⎧𝑠 (𝜆 − 1 − {{{{{ {{{{{ ∫ 𝑓s(1 − 𝜇)𝑑𝜇 ⎨ ⎩ ) if 𝜆 ≥ + 1 if 1 ≤ 𝜆 < otherwise + 1 (22.121.8) Here s is the nominal tensile cutoff stress and 𝐸 is the stiffness coefficient relating a change in principal stretch to a corresponding change in nominal stress. The function 𝑓s(≤ 0) gives the nominal compressive stress as a function of the strain in compression for the second and all subsequent load cycles and is supplied by the user. To apply the formulas in the previous section, we require E = 𝜆𝑖 𝜏𝑖𝑖 𝜕𝑤 𝜕𝜆𝑖 = if 𝜆𝑖 ≥ + 1 𝐸𝜆𝑖(𝜆𝑖 − 1) if 1 ≤ 𝜆𝑖 < 𝜆𝑖𝑓𝑠(1 − 𝜆𝑖) otherwise ⎧𝑠𝜆𝑖 {{{ ⎨ {{{ ⎩ + 1 (22.121.9) Proceeding with the constitutive tensor, we have Material Models LS-DYNA Theory Manual 𝜆𝑗 𝜕𝜏𝑖𝑖 𝜕𝜆𝑗 = 𝛿𝑖𝑗 ⎧𝑠𝜆𝑖 {{{ ⎨ {{{ ⎩ 𝐸𝜆𝑖(2𝜆𝑖 − 1) if 1 ≤ 𝜆𝑖 < 𝜆𝑖(𝑓𝑠(1 − 𝜆𝑖) − 𝜆𝑖𝑓 ′𝑠(1 − 𝜆𝑖)) otherwise if 𝜆𝑖 ≥ + 1 + 1 (22.121.10) 22.121.3 Modeling of the Hysteresis The hyperelastic part of the Cauchy stress is scaled by a factor 𝜅 given by where 𝜅 = , 𝐸̅̅̅̅ 𝐸 = ∫ 𝐽𝛔: 𝑑𝛆, is the stored energy in the material and 𝐸̅̅̅̅ = 𝐸maxexp(−𝛽(𝑡 − 𝑠)). (22.121.11) (22.121.12) (22.121.13) Here 𝑠 stands for the time point when E has its maximum 𝐸max in the interval [0, 𝑡]. The factor κ is introduced to model the hysteresis that characterizes this material (and material 57). The decay coefficient 𝛽 is introduced to get a reloading curve similar to the original loading curve. This factor κ is treated as a constant in the determination of the tangent stiffness matrix. 22.121.4 Viscous Stress In addition to the hyperelastic stress described above, a viscous stress is added. Converting to Voigt notation, this stress can be written 𝛔 = 𝐂𝐃, (22.121.14) where 𝛔 denotes Cauchy stress, 𝐃 is the rate-of-deformation and 𝐂 is an isotropic constitutive matrix representing the viscosity. In element m, the constitutive matrix depends on the element deformation according to 𝐂 = 𝑑𝑚 𝐂0, (22.121.15) where 𝑑𝑚 is the diameter5 of element m and 𝐂0 is a constitutive matrix that depends only on the material parameters. Following material models 177 and 178 we use the following material tangent stiffness for this stress contribution 5 Experiments indicate that d(cid:2923) is the smallest dimension of the element. LS-DYNA Theory Manual Material Models 𝐂mat = 𝛽Δ𝑡 𝐂, (22.121.16) where 𝛾 and 𝛽 are parameters in the Newmark scheme and Δ𝑡 is the time step. 22.121.5 Viscoelastic Stress Contribution An optional viscoelastic stress contribution can be added. The evolution of this stress in time can be stated as where ∇, ∇ = 𝐸d𝑠𝑖𝑗 𝜎𝑖𝑗 ∇ = 𝐷𝑖𝑗 − 𝛽1𝑠𝑖𝑗. 𝑠𝑖𝑗 (22.121.17) (22.121.18) Here 𝐸d and 𝛽1 are material constants, 𝐷𝑖𝑗 is the rate-of-deformation tensor and ∇ stands for an objective rate. Referring to material models 177 and 178, we state that the tangent stiffness modulus for this stress contribution can be written 𝐶𝑖𝑗𝑘𝑙 = 𝐸d (𝛿𝑖𝑘𝛿𝑗𝑙 + 𝛿𝑖𝑙𝛿𝑗𝑘). (22.121.19) This stress acts only in the direction of the principal stretches. Hence the tangent modulus is formed in the principal basis, modified to account for this condition and then transformed back to the global frame of reference. 22.121.6 Stress Corresponding to First Load Cycle We define a contribution to the principal Kirchhoff stress as 1 𝜏𝑖𝑖 E = 𝜆𝑖{𝑔s(1 − 𝜆𝑖) − 𝑓s(1 − 𝜆𝑖)}𝜉 . (22.121.20) When the damage is isotropic the factor 𝜉 is given by 𝜉 = max (0,1 − 𝜀h 0.0001 + 𝜀m ). (22.121.21) where 𝜀h is the damage parameter that is initially zero and 𝜀m is the maximum compressive volumetric strain during the entire simulation thus far. Damage evolves when the material is in compression and unloads Δ𝜀h = { max(0, Δ𝐽) otherwise if 𝐽 ≥ 1 , (22.121.22) where 𝐽 is the jacobian of the deformation. The first load cycle will result in a total stress that follows load curve 𝑔𝑠 since there is no damage. After a complete load cycle, i.e., unloading has occurred, the material is completely damaged, i.e., 𝜀h ≈ 𝜀m, and the Material Models LS-DYNA Theory Manual nominal stress will for the second and subsequent load cycles be given by the load curve 𝑓s. In the orthotropic case the principal Kirchhoff stress contribution is instead given by 1 𝜏𝑖𝑖 E = 𝜆𝑖{𝑔𝑠(1 − 𝜆𝑖) − 𝑓𝑠(1 − 𝜆𝑖)}𝜉𝑖. (22.121.23) For the damage to be orthotropic we introduce a symmetric and positive definite 𝑖𝑗. This tensor is initially the zero tensor corresponding to no damage. damage tensor 𝜀h The evolution of damage begins with a half step Jaumann rotation of the tensor to maintain objectivity. After that the local increment is performed. As for the isotropic case, damage evolves in compression in combination with unloading. We introduce the local damage increment as Δ𝜀loc if 𝜆𝑖 ≥ 1 𝑖𝑗 = 𝛿𝑖𝑗 { max(0, Δ𝜆𝑖) otherwise , (22.121.24) which is a diagonal tensor. The global damage tensor increment is given by 𝑖𝑗 = 𝑞𝑖𝑘𝑞𝑗𝑙Δ𝜀loc 𝑘𝑙 , Δ𝜀ℎ (22.121.25) which is used to increment the damage tensor 𝜀ℎ 𝑘𝑙 𝑞𝑘𝑖𝑞𝑙𝑖𝜀ℎ ⎟⎞. 0.0001 + 𝜀m⎠ ⎜⎛0,1 − ⎝ 𝜉𝑖 = max 𝑖𝑗. The factor 𝜉𝑖 is now given by (22.121.26) where the quantity 𝜀m in the orthotropic case is the maximum compressive principal strain in any direction during the simulation thus far. As for the isotropic case, the material is completely damaged after one load cycle and reloading will follow load curve 𝑓s. In addition, the directions corresponding to no loading will remain unaffected. The factors 𝜉 and 𝜉𝑖 are treated as constants in the determination of the tangent stiffness so the contribution is regarded as hyperelastic and follows the exposition given in Section 19.179.1. The reason for not differentiating the coefficients 𝜅, 𝜉 and 𝜉𝑖 is that they are always non-differentiable. Their changes depend on whether the material is loaded or unloaded, i.e., the direction of the load. Even if they were differentiable their contributions would occasionally result in a non-symmetric tangent stiffness matrix and any attempt to symmetrize this would probably destroy its properties. After all, we believe that the one-dimensional nature and simplicity of this foam will be enough for good convergence properties even without differentiating these coefficients. LS-DYNA Theory Manual Material Models 22.122 Material Model 181: Simplified Rubber/Foam Material type 181 in LS-DYNA is a simplified “quasi”-hyperelastic rubber or foam model defined by a single uniaxial load curve or by a family of curves at discrete strain rates. The term “quasi” is used because there is really no strain energy function for determining the stresses used in this model. Rather the stress response mimics the gradient of the strain energy potential in the Ogden rubber . For deriving the tangent stiffness matrix we use the formulas as if a strain energy function were present, with appropriate modifications. This model is equipped with various features related to dissipation and damage, but not all of those are described in detail. 𝐴 𝑔(𝜆) = 𝑃/𝐴 𝜆 = 𝜆1 = 𝑙/𝐿 𝜆2 = 𝜆3 = 𝑑/𝐷 𝐷 22-122 Uniaxial test parameters. 22.122.1 Hyperelasticity Using the Principal Stretch Ratios A hyperelastic constitutive law is determined by a strain energy function that we assume is expressed in terms of the principal stretches, i.e., 𝑊 = 𝑊(𝜆1, 𝜆2, 𝜆3). To obtain the Cauchy stress 𝜎𝑖𝑗 this is first calculated in the principal basis after which it is transformed back to the “base frame”, or standard basis. The complete set of formulas is given by Crisfield [1997] and is for the sake of completeness recapitulated here. For the following discussion we refer to figure 22-122 The principal Kirchhoff stress components are given by E = 𝜆𝑖 𝜏𝑖𝑖 𝜕𝑊 𝜕𝜆𝑖 (no sum), (22.122.1) that are transformed to the standard basis using the standard formula Material Models LS-DYNA Theory Manual E. 𝜏𝑖𝑗 = 𝑞𝑖𝑘𝑞𝑗𝑙𝜏𝑘𝑙 (22.122.2) The 𝑞𝑖𝑗 are the components of the orthogonal tensor containing the eigenvectors of the principal basis. The Cauchy stress is then given by 𝜎𝑖𝑗 = 𝐽−1𝜏𝑖𝑗, (22.122.3) where 𝐽 = 𝜆1𝜆2𝜆3 is the relative volume change. Now, the Ogden strain energy potential results in a Kirchhoff stress on the form 𝐸 = 𝑓 (𝜆̃𝑖) + 𝐾𝑚(𝐽 − 1) − 𝜏𝑖𝑖 ∑ 𝑓 (𝜆̃𝑘) 𝑘=1 (22.4) for a (large) bulk modulus 𝐾𝑚 and where 𝜆̃𝑖 = 𝜆𝑖/𝐽1/3 are the isochoric stretches. In the Ogden material, 𝑓 has a specific form a priori that requires a least square approximation for fitting test data. This is of course a restriction and the idea in material 181 is to let 𝑓 be determined directly from input data. The ansatz for the compressible foam option is to let 𝐸 = 𝑓 (𝜆𝑖) − 𝑓 (𝐽 𝜏𝑖𝑖 − 𝜈 1−2𝜈) (22.5) for a given Poisson’s ratio 𝜈, a decision that will be made clear below. So assume that 𝑔(𝜆) is the curve providing the engineering stress as function of stretch in a uniaxial test, see figure 22-122, then the principal Kirchhoff stresses are 𝐸 = 𝜆𝑔(𝜆) 𝜏11 𝐸 = 0 𝐸 = 𝜏33 𝜏22 What follows is the determination of the internal function 𝑓 for the rubber and foam option. (22.6) 22.122.1.1 For incompressibility we deduce that the principal stretches are Determination of f, rubber option which coincide with the isochoric counterparts. Using these expressions when equating (22.4) and (22.6), one must determine 𝑓 from 𝜆1 = 𝜆 𝜆2 = 𝜆3 = 𝜆−1/2 (22.7) (𝑓 (𝜆) − 𝑓 (𝜆−1/2)) + 𝐾𝑚(𝐽 − 1) (𝑓 (𝜆−1/2) − 𝑓 (𝜆)) + 𝐾𝑚(𝐽 − 1). 𝜆𝑔(𝜆) = 0 = By subtracting these two equations to eliminate the influence of the pressure we get (22.8) that can be rewritten as 𝜆𝑔(𝜆) = 𝑓 (𝜆) − 𝑓 (𝜆 −1 2) 𝑓 (𝜆) = 𝜆𝑔(𝜆) + 𝑓 (𝜆−1/2). This in turn can be recursively expanded as (22.9) (22.10) LS-DYNA Theory Manual Material Models 𝑓 (𝜆) = 𝜆𝑔(𝜆) + 𝜆−1/2𝑔(𝜆−1/2) + 𝜆1/4𝑔(𝜆1/4) + ⋯ + 𝑓 (𝜆(−1/2)𝑛 ) (22.11) ) and by letting 𝑛 be large enough the function 𝑓 can be determined since the last term tends to zero. Determination of f, foam option 22.122.1.2 Similarly, for a given Poisson’s ratio 𝜈, the principal stretches in a uniaxial tension test are 𝜆1 = 𝜆 𝜆2 = 𝜆3 = 𝜆−𝜈 (22.12) and using (22.5) and (22.6) the equation to solve is now (22.13) Note that the equation corresponding to the second of (22.6) vanishes because of the ansatz in (22.5). The same technique as for the rubber option is used, recursive expansion gives 𝜆𝑔(𝜆) = 𝑓 (𝜆) − 𝑓 (𝜆−𝜈) ) + ⋯ + 𝑓 (𝜆(−𝜈)𝑛 which for a large 𝑛 gives a sufficiently accurate representation of 𝑓 . 𝑓 (𝜆) = 𝜆𝑔(𝜆) + 𝜆−𝜈𝑔(𝜆−𝜈) + 𝜆𝜈2 𝑔(𝜆𝜈2 ) (22.14) 22.122.2 Some Remarks 22.122.2.1 Strain rates The function 𝑓 introduced in the previous section depends not only on the stretches but for some choices of input also on the strain rate. In this case each test curve 𝑔𝑖(𝜆) corresponding to a particular strain rate 𝜀̇𝑖 is converted to an internal function 𝑓𝑖(𝜆) following the procedure described in the previous section. These internal functions are then used for determining the response for a given strain rate 𝜀̇ by interpolation. Strain rates are treated in various ways depending on user defined parameters and we refer to Section and the Keyword Manual for more info. 22.122.2.2 Modeling of the Frequency Independent Damping An elastic-plastic stress 𝜎𝑑 is added to model the frequency independent damping properties of rubber. This stress is deviatoric and determined by the shear modulus 𝐺 and the yield stress 𝜎𝑌. This part of the stress is updated incrementally as 𝑛 + 2𝑮𝑰dev𝛥𝜺, (22.122.15) 𝑛+1 = 𝝈𝑑 𝝈̃𝑑 where 𝛥𝜺 is the strain increment. The trial stress is then radially scaled (if necessary) to the yield surface according to 𝑛+1 = 𝜎̃𝑑 𝜎𝑑 𝑛+1min (1, 𝜎𝑌 𝜎eff ), (22.122.16) where 𝜎eff is the effective von Mises stress for the trial stress 𝜎̃𝑑 𝑛+1. Material Models LS-DYNA Theory Manual 22.123 Material Model 187: Semi-Analytical Model for the Simulation of Polymers 22.123.1 Material law formulation Choice of a yield surface formulation All plastics are to some degree anisotropic. The anisotropic characteristic can be due to fibre reinforcement, to the moulding process or it can be load induced in which case the material is at least initially isotropic. Therefore a quadratic form in the stress tensor is often used to describe the yield surface. We restrict the scope of this work to isotropic formulations. However, the choice of this yield surface was made in view of later anisotropic generalisations. In the isotropic case the most general quadratic yield surface can be written as 𝑓 = 𝛔T𝐅𝛔 + 𝐁𝛔 + 𝐹0 ≤ 0, (22.123.1) where 𝛔 = ⎝ ⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎛ ⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎛ ⎜⎜⎜⎜⎜⎜⎜⎜⎜⎜⎛ ⎝ , ⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎞ σ𝑥𝑥 σ𝑦𝑦 σ𝑧𝑧 σ𝑥𝑦 σ𝑦𝑧 σ𝑧𝑥⎠ 𝐹11 𝐹12 𝐹12 𝐹12 𝐹11 𝐹12 𝐹12 𝐹12 𝐹11 𝐹1 𝐹1 𝐹1 , 𝐅 = ⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎞ 𝐹44 𝐹44⎠ 𝐹44 Some restrictions apply to the choice of the coefficients. The existence of a stress-free state and the equivalence of pure shear and biaxial tension/compression require respectively 0⎠ ⎟⎟⎟⎟⎟⎟⎟⎟⎟⎟⎞ 𝐁 = (22.123.2) ⎝ . 𝐹0 ≤ 0 and 𝐹44 = 2(𝐹11 − 𝐹12). (22.123.3) Although 4 independent coefficients remain in the expression for the isotropic yield surface at this point, however the yield condition is not affected if all coefficients are multiplied by a constant. Consequently only 3 coefficients can be freely chosen and 3 experiments under different states of stress can be fitted by this formulation. LS-DYNA Theory Manual Material Models Figure 22.1. Recommended tests for material data in SAMP Without loss of generality the expression for the yield surface can be reformulated in terms of the first two stress invariants: pressure and von Mises stress: 𝑝 = − σ𝑥𝑥 + σ𝑦𝑦 + σ𝑧𝑧 , σvm = √ ((σ𝑥𝑥 + 𝑝)2 + (σ𝑦𝑦 + 𝑝) + (σ𝑧𝑧 + 𝑝)2 + 2σ𝑥𝑦 2 + 2σ𝑦𝑧 2 ) 2 + 2σ𝑧𝑥 . (22.123.4) The expression for the yield surface then becomes 𝑓 = σvm 2 − 𝐴0 − 𝐴1𝑝 − 𝐴2𝑝2 ≤ 0, (22.123.5) and identification of the coefficients gives 𝐴0 = −𝐹0 , 𝐴1 = 3𝐹1 and 𝐴2 = 9(1 − 𝐹11), (22.123.6) or equivalently 𝐹0 = −𝐴0, 𝐹1 = 𝐴1 , 𝐹11 = 1 − 𝐴2 , 𝐹44 = 3 and 𝐹12 = 𝐹11 − 𝐹44 = − ( + 𝐴2 ). (22.123.7) Since there is no loss of generality, the simpler formulation in invariants is adopted from this point on. In principle the coefficients of the yield surface can now be determined from 3 experiments. Typically we would perform uniaxial tension, uniaxial compression and simple shear tests: This allows computation of the coefficients in function of the test results: 3σs 2 = 𝐴0 2 = 3σs σt 2 − 𝐴1 2 = 3σs σc 2 + 𝐴1 σt σc + 𝐴2 + 𝐴2 ⎫ }}}} σt }}}} σc 9 ⎭ ⎬ ⇒ ⎧𝐴0 = 3σs {{{{ 𝐴1 = 9σs {{{{ 𝐴2 = 9 ( ⎨ ⎩ ) 2 ( σc − σt σcσt σcσt − 3σs σcσt ) . (22.123.8) Alternatively we can also compute the coefficients relating to the formulation in stress space: Material Models LS-DYNA Theory Manual 𝐹1 = 𝐹0 ( − 𝐹0 + 𝐹1𝜎t + 𝐹11σt 2 = 0 𝐹0 − 𝐹1σc + 𝐹11σc 2 = 0 𝐹0 + 𝐹44σs 2 = 0 ⎫ }}}}} }}}}} ⎬ ⎭ ⇒ ⎧ {{{{{ {{{{{ ⎨ ⎩ 𝐹11 = − 𝐹44 = − σc 𝐹0 σtσc 𝐹0 σs σt ) . (22.123.9) Both are easily seen to be equivalent. Conditions for convexity of the yield surface Usually the yield surface is required to be convex, i.e. 𝑓 (σ1) ≤ 0 }⎫ 𝑓 (σ2) ≤ 0 0 ≤ α ≤ 1⎭}⎬ ⇒ 𝑓 (ασ1 + (1 − α)σ2) ≤ 0. (22.123.10) The second derivative of 𝑓 is computed as 𝑓 = 𝛔T𝐅𝛔 + 𝐁𝛔 + 𝐹0 → ∂2𝑓 ∂σ2 = 2𝐅 (22.123.11) A sufficient condition for convexity in 6D stress space is then that the matrix F should be positive semidefinite. This means all eigenvalues of F should be positive or zero. The conditions for convexity will now be examined in physical terms for two cases: plane stress and general 3D. The plane stress case In the plane stress case the yield condition reduces to: 𝑓 = 𝛔T𝐅𝛔 + 𝐁𝛔 + 𝐹0, where ⎟⎞, 0⎠ And convexity requires the eigenvalues of F to be non-negative: 𝐹11 𝐹12 𝐹12 𝐹11 𝐹44⎠ ⎟⎟⎞ 𝐁 = ⎟⎟⎞ 𝐅 = 𝐹1 𝐹1 σ𝑥𝑥 σ𝑦𝑦 σ𝑥𝑦⎠ ⎜⎜⎛ ⎝ ⎜⎜⎛ ⎝ 𝛔 = ⎜⎛ ⎝ 𝐹11 + 𝐹12 ≥ 0 𝐹11 − 𝐹12 ≥ 0 𝐹44 ≥ 0 }⎫ ⎭}⎬ ⇒ { 2 ≥ σtσc 4σs −𝐹0 ≥ 0 . (22.123.12) (22.123.13) (22.123.14) The 3D case In the full 3D case, the convexity condition is generally more stringent. Again we require the eigenvalues of F to be non-negative, where F is now the full 6 by 6 matrix: 𝐹11 + 2𝐹12 ≥ 0 𝐹11 − 𝐹12 ≥ 0 𝐹44 ≥ 0 }⎫ ⎭}⎬ ⇒ { 2 ≥ σtσc 3σs −𝐹0 ≥ 0 . (22.123.15) LS-DYNA Theory Manual Material Models Leading to σs ≥ √σtσc √3 > √σtσc . (22.123.16) Alternatively a yield surface containing a linear rather than a quadratic term was implemented in SAMP-1. 𝑓 = σvm − 𝐴0 − 𝐴1𝑝 − 𝐴2𝑝2 ≤ 0. (22.123.17) As it will be difficult in general to guarantee a reasonable flow behaviour from three independent measurements in shear, tension and compression, a simplified flow rule has been implemented as the default in SAMP-1. The generally non-associated flow surface is given as: 𝑔 = σvm 2 + α𝑝2. This flow rule is associated if: 𝐴1 = 0, 𝐴2 = −α And clearly leads to a constant value for the plastic Poisson ratio: (= cte). ν𝑝 = 9 − 2α 18 + 2α ⇒ α = 1 − 2ν𝑝 1 + ν𝑝 . Plausible flow behaviour just means that: 0 ≤ α ≤ ⇒ 0 ≤ ν𝑝 ≤ 0.5. (22.123.18) (22.123.19) (22.123.20) (22.123.21) In SAMP-1 the value of the plastic Poisson coefficient is given by the user, either as a constant or as a load curve in function of the uniaxial plastic strain. This allows adjusting the flow rule of the material to measurements of transversal deformation during uniaxial tensile or compressive testing. This can be important for plastics since often a non-isochoric behaviour is measured. Material Models LS-DYNA Theory Manual Figure 22.2. Influence of the flow rule on the plastic Poisson ratio The possible values for the plastic Poisson ratio and the resulting flow behaviour are illustrated in Figure 22.2. In SAMP-1 the formulation is slightly modified and based on a flow rule given as: The plastic strain rate computation is not normalized: 𝑔′ = √σvm 2 + α𝑝2. ε̇p = λ̇ ∂𝑔′ ∂σ . The volumetric and deviatoric plastic strain rates in this case are given as : ε̇vp = λ̇ (−2α𝑝) 2𝑔′⁄ = ε̇dp = λ̇ 3s 2𝑔′⁄ = λ̇ (−2α𝑝) , 2 + 4α𝑝2 √4σvm λ̇ 3s , √4σvm 2 + 4α𝑝2 (22.123.22) (22.123.23) (22.123.24) which amounts to a different definition of the plastic consistency parameter which of course has to be considered when equivalent plastic strain values are computed. 22.123.2 Hardening formulation The hardening formulation is the attractive part of SAMP-1. The formulation is fully tabulated and consequently the user can directly input measurement results from uniaxial tension, uniaxial compression and simple shear tests in terms of load curves giving the yield stress as a function of the corresponding plastic strain. No fitting of coefficients is required. The test results that are reflected in the load curves will be used exactly by SAMP-1 without fitting to any analytical expression. Consequently the LS-DYNA Theory Manual Material Models Figure 22.3. Tensile hardening curve from dynamic tensile tests hardening will be dependent upon the state of stress and not only upon the plastic strain. 22.123.3 Rate effects Plastics are usually highly rate dependent. A proper viscoplastic consideration of the rate effects is therefore important in the numerical treatment of the material law. Data to determine the rate dependency are based on uniaxial dynamic testing. If dynamic tests are available, then the load curve defining the yield stress in uniaxial tension is simply replaced by a table definition containing multiple load curves corresponding to different values of the plastic strain rate. This is illustrated in the Figure 22.3. 22.123.4 Damage and failure Numerous damage models can be found in the literature. Probably the simplest concept is elastic damage where the damage parameter (usually written as 𝑑) is a function of the elastic energy and effectively reduces the elastic modulus of the material. In the case of ductile damage, 𝑑 is a function of plastic straining and affects the yield stress rather than the elastic modulus. This is equivalent to plastic softening. In more sophisticated damage models, d depends on both the plastic straining and the elastic energy (and maybe other factors) and effects yield stress as well as elastic modulus. A simple damage model was added to the SAMP-1 material law where the damage parameter d is a function of plastic strain only. A load curve must be provided by the user giving d as a function of the (true) plastic strain under uniaxial tension. The value of the critical damage Dc leading to rupture is then the only other required additional input. The implemented damage model is isotropic. Material Models LS-DYNA Theory Manual Figure 22.4. Damage parameter from uniaxial tensile test The implemented model then uses the notion of effective cross section, which is the true cross section of the material minus the cracks that have developed. We will use the following notation: 𝐴0 → undeformed cross section 𝐴 → deformed or current cross section 𝐴0 → undeformed cross section We define the effective stress as the force divided by the effective cross section: σ = σeff = , 𝐴eff = 𝐴(1 − 𝑑) = 1 − 𝑑 , which allows defining an effective yield stress: σy,eff = σy 1 − 𝑑 . (22.25) (22.26) LS-DYNA Theory Manual Material Models 22.124 Material Model 196: General Spring Discrete Beam If TYPE = 0, elastic behavior is obtained. In this case, if the linear spring stiffness is used, the force, 𝐹, is given by: 𝐹 = 𝐹0 + 𝐾Δ𝐿 + 𝐷Δ𝐿̇, (22.124.1) but if the load curve ID is specified, the force is then given by: 𝐹 = 𝐹0 + 𝐾 𝑓 (Δ𝐿) [1 + 𝐶1 ⋅ Δ𝐿̇ + 𝐶2 ⋅ sgn(Δ𝐿̇)ln (max {1. , + 𝑔(Δ𝐿)ℎ(Δ𝐿̇). ∣Δ𝐿̇∣ 𝐷𝐿𝐸 })] + 𝐷Δ𝐿̇ (22.124.2) In these equations, Δ𝐿 is the change in length Δ𝐿 = current length − initial length. (22.124.3) If TYPE = 1, inelastic behavior is obtained. In this case, the yield force is taken from the load curve: 𝐹Y = 𝐹y(Δ𝐿plastic), where 𝐿plastic is the plastic deflection. A trial force is computed as: and is checked against the yield force to determine F: 𝐹T = 𝐹n + KΔ𝐿̇Δ𝑡, 𝐹 = {𝐹Y if 𝐹T > 𝐹Y 𝐹T if 𝐹T ≤ 𝐹Y. (22.124.4) (22.124.5) (22.124.6) The final force, which includes rate effects and damping, is given by: 𝐹𝑛+1 = 𝐹 ⋅ [1 + 𝐶1 ⋅ Δ𝐿̇ + 𝐶2 ⋅ sgn(Δ𝐿̇)ln (max {1. , + 𝑔(Δ𝐿)ℎ(Δ𝐿̇). ∣Δ𝐿̇∣ 𝐷𝐿𝐸 })] + 𝐷Δ𝐿̇ (22.124.7) Unless the origin of the curve starts at (0,0), the negative part of the curve is used when the spring force is negative where the negative of the plastic displacement is used to interpolate, 𝐹y. The positive part of the curve is used whenever the force is positive. The cross sectional area is defined on the section card for the discrete beam elements, See *SECTION_BEAM. The square root of this area is used as the contact thickness offset if these elements are included in the contact treatment. LS-DYNA Theory Manual Equation of State Models 23 Equation of State Models LS-DYNA has 10 equation of state models which are described in this section. 1. 2. 3. 4. 5. 6. 7. 8. 9. 10. Linear Polynomial JWL High Explosive Sack “Tuesday” High Explosive Gruneisen Ratio of Polynomials Linear Polynomial With Energy Deposition Ignition and Growth of Reaction in High Explosives Tabulated Compaction Tabulated Propellant-Deflagration The forms of the first five equations of state are given in the KOVEC user’s manual [Woodruff 1973] as well as below. 23.1 Equation of State Form 1: Linear Polynomial This polynomial equation of state, linear in the internal energy per initial volume, 𝐸, is given by 𝑝 = 𝐶0 + 𝐶1𝜇 + 𝐶2𝜇2 + 𝐶3𝜇3 + (𝐶4 + 𝐶5𝜇 + 𝐶6𝜇2)𝐸 Here 𝐶0, 𝐶1, 𝐶2, 𝐶3, 𝐶4, 𝐶5 and 𝐶6 are user defined constants and 𝜇 = − 1. (23.1.1) (23.1.2) where 𝑉 is the relative volume. In expanded elements, the coefficients of 𝜇2 are set to zero, i.e., 𝐶2 = 𝐶6 = 0. (23.1.3) Equation of State Models LS-DYNA Theory Manual The linear polynomial equation of state may be used to model gas with the gamma law equation of state. This may be achieved by setting: and 𝐶0 = 𝐶1 = 𝐶2 = 𝐶3 = 𝐶6 = 0, 𝐶4 = 𝐶5 = 𝛾 − 1, where 𝛾 is the ratio of specific heats. The pressure is then given by: Note that the units of 𝐸 are the units of pressure. 𝑝 = (𝛾 − 1) 𝜌0 𝐸. (23.1.4) (23.1.5) (23.1.6) 23.2 Equation of State Form 2: JWL High Explosive The JWL equation of state defines pressure as a function of relative volume, 𝑉, and internal energy per initial volume, 𝐸, as 𝑝 = 𝐴 (1 − 𝑅 1𝑉 ) 𝑒−𝑅 1𝑉 + 𝐵 (1 − 𝑅 2𝑉 ) 𝑒−𝑅 2𝑉 + 𝜔𝐸 , (23.2.7) where 𝜔, A, 𝐵, 𝑅1 and 𝑅2 are user defined input parameters. The JWL equation of state is used for determining the pressure of the detonation products of high explosives in applications involving metal accelerations. Input parameters for this equation are given by Dobratz [1981] for a variety of high explosive materials. This equation of state is used with the explosive burn (material model 8) material model which determines the lighting time for the explosive element. 23.3 Equation of State Form 3: Sack “Tuesday” High Explosives Pressure of detonation products is given in terms of the relative volume, 𝑉, and internal energy per initial volume, 𝐸, as [Woodruff 1973]: 𝐴 3 𝑉 𝐴1 where 𝐴1, 𝐴2, 𝐴3, 𝐵1 and 𝐵2 are user-defined input parameters. 𝑒−𝐴 2𝑉 (1 − 𝐵1 𝐵2 ) + 𝑝 = 𝐸, (23.3.8) LS-DYNA Theory Manual Equation of State Models This equation of state is used with the explosive burn (material model 8) material model which determines the lighting time for the explosive element. 23.4 Equation of State Form 4: Gruneisen The Gruneisen equation of state with cubic shock velocity-particle velocity defines pressure for compressed material as )𝜇 − 𝑎 𝜌0𝐶2𝜇[1 + (1 − 𝜇 2] 𝑝 = 𝛾0 𝜇 2 𝜇 + 1 − 𝑆3 𝜇 3 (𝜇 + 1)2] [1 − (𝑆1 − 1)𝜇 − 𝑆2 2 + (𝛾0 + 𝛼𝜇)𝐸, (23.4.9) where 𝐸 is the internal energy per initial volume, 𝐶 is the intercept of the 𝑢s − 𝑢p curve, 𝑆1, 𝑆2, and 𝑆3 are the coefficients of the slope of the 𝑢s − 𝑢p curve, 𝛾0 is the Gruneisen gamma, and a is the first order volume correction to 𝛾0. Constants 𝐶, 𝑆1, 𝑆2, 𝑆3, 𝛾0 and 𝑎 are user defined input parameters. The compression is defined in terms of the relative volume, 𝑉, as: 𝜇 = − 1. For expanded materials as the pressure is defined by: 𝑝 = 𝜌0 𝐶 2𝜇 + (𝛾0 + 𝛼𝜇)𝐸. 23.5 Equation of State Form 5: Ratio of Polynomials The ratio of polynomials equation of state defines the pressure as 𝑝 = 𝐹1 + 𝐹2𝐸 + 𝐹3𝐸2 + 𝐹4𝐸3 𝐹5 + 𝐹6𝐸 + 𝐹7𝐸2 (1 + 𝛼𝜇), where 𝐹𝑖 = ∑ 𝐴𝑖𝑗𝑚𝑗 𝑗= 0 , 𝑛 = 4 if 𝑖 < 3, 𝑛 = 3 if 𝑖 ≥ 3 𝜇 = 𝜌0 − 1 . (23.4.10) (23.4.11) (23.5.12) (23.5.13) (23.5.14) Equation of State Models LS-DYNA Theory Manual In expanded zoned 𝐹1 is replaced by 𝐹′1 = 𝐹1 + 𝛽𝜇2 Constants 𝐴𝑖𝑗, 𝛼, and 𝛽 are user input. 23.6 Equation of State Form 6: Linear With Energy Deposition This polynomial equation of state, linear in the internal energy per initial volume, 𝐸, is given by 𝑝 = 𝐶0 + 𝐶1𝜇 + 𝐶2𝜇2 + 𝐶3𝜇3 + (𝐶4 + 𝐶5𝜇 + 𝐶6𝜇2)𝐸, Here 𝐶0, 𝐶1, 𝐶2, 𝐶3, 𝐶4, 𝐶5 and 𝐶6 are user defined constants and 𝜇 = − 1, (23.6.15) (23.6.16) where 𝑉 is the relative volume. In expanded elements, we set the coefficients of 𝜇2 to zero, i.e., 𝐶2 = 𝐶6 = 0. (23.6.17) Internal energy, 𝐸, is increased according to an energy deposition rate versus time curve whose ID is defined in the input. 23.7 Equation of State Form 7: Ignition and Growth Model A JWL equation of state defines the pressure in the unreacted high explosive as 𝑃𝑒 = 𝐴𝑒 (1 − 𝜔𝑒 𝑅1𝑒𝑉𝑒 ) 𝑒−𝑅1𝑒𝑉𝑒 + 𝐵𝑒 (1 − 𝜔𝑒 𝑅2 𝑒𝑉𝑒 ) 𝑒−𝑅2 𝑒𝑉𝑒 + 𝜔𝑒𝐸 𝑉𝑒 , (23.7.18) where 𝑉𝑒 is the relative volume, 𝐸𝑒 is the internal energy, and the constants 𝐴𝑒, 𝐵𝑒, 𝜔𝑒, 𝑅1𝑒 and 𝑅2𝑒 are input constants. Similarly, the pressure in the reaction products is defined by another JWL form 𝑃𝑝 = 𝐴𝑝 (1 − 𝜔𝑝 𝑅1𝑝 𝑉𝑝 ) 𝑒−𝑅1𝑝𝑉𝑝 + 𝐵𝑝 (1 − 𝜔𝑒 𝑅2 𝑝𝑉𝑝 ) 𝑒−𝑅2 𝑝 𝑉𝑝 + 𝜔 𝑝𝐸 . 𝑉𝑝 (23.7.19) The mixture of unreacted explosive and reaction products is defined by the fraction reacted 𝐹 (𝐹 = 0 implies no reaction, 𝐹 = 1 implies complete conversion from explosive to products). The pressures and temperature are assumed to be in equilibrium, and the relative volumes are assumed to be additive: LS-DYNA Theory Manual Equation of State Models 𝑉 = (1 − 𝐹)𝑉𝑒 + 𝐹𝑉𝑝. (23.7.20) The rate of reaction is defined as = 𝐼(FCRIT − 𝐹)𝑦(𝑉𝑒 ∂𝐹 ∂𝑡 where 𝐼, 𝐺, 𝐻, 𝑥, 𝑦, 𝑧 and 𝑚 (generally 𝑚 = 0) are input constants. −1 − 1)] + 𝐻(1 − 𝐹)𝑦𝐹𝑥𝑃𝑧(𝑉𝑝 [1 + 𝐺(𝑉 𝑒 −1 − 1) −1 − 1) , (23.7.21) The JWL equations of state and the reaction rates have been fitted to one- and two-dimensional shock initiation and detonation data for four explosives: PBX-9404, RX-03-BB, PETN, and cast TNT. The details of calculational method are described by Cochran and Chan [1979]. The detailed one-dimensional calculations and parameters for the four explosives are given by Lee and Tarver [1980]. Two-dimensional calculations with this model for PBX 9404 and LX-17 are discussed by Tarver and Hallquist [1981]. 23.8 Equation of State Form 8: Tabulated Compaction Pressure is positive in compression, and volumetric strain 𝜀𝑉 is positive in tension. The tabulated compaction model is linear in internal energy per unit volume. Pressure is defined by 𝑝 = 𝐶(𝜀𝑉) + 𝛾𝑇(𝜀𝑉)𝐸, (23.8.22) during loading (compression). Unloading occurs at a slope corresponding to the bulk modulus at the peak (most compressive) volumetric strain, as shown in Figure 23.1. Reloading follows the unloading path to the point where unloading began, and then continues on the loading path described by Equation (23.8.22). 23.9 Equation of State Form 9: Tabulated The tabulated equation of state model is linear in internal energy. Pressure is defined by 𝑝 = 𝐶(𝜀𝑉) + 𝛾𝑇(𝜀𝑉)𝐸, (23.9.23) The volumetric strain 𝜀𝑉 is given by the natural algorithm of the relative volume. Up to 10 points and as few as 2 may be used when defining the tabulated functions. The pressure is extrapolated if necessary. Loading and unloading are along the same curve unlike equation of state form 8. Equation of State Models LS-DYNA Theory Manual kεA εA kεC εC V) kεB εB (-ε Volumetric Strain Figure 23.1. Pressure versus volumetric strain curve for equation of state form 8 with compaction. In the compacted states, the bulk unloading modulus depends on the peak volumetric strain. 23.10 Equation of State Form 10: Propellant-Deflagration A deflagration (burn rate) reactive flow model requires an unreacted solid equation-of-state, a reaction product equation-of-state, a reaction rate law and a mixture rule for the two (or more) species. The mixture rule for the standard ignition and growth model [Lee and Tarver 1980] assumes that both pressures and temperatures are completely equilibrated as the reaction proceeds. However, the mixture rule can be modified to allow no thermal conduction or partial heating of the solid by the reaction product gases. For this relatively slow process of airbag propellant burn, the thermal and pressure equilibrium assumptions are valid. The equations-of-state currently used in the burn model are the JWL, Gruneisen, the van der Waals co-volume, and the perfect gas law, but other equations-of-state can be easily implemented. In this propellant burn, the gaseous nitrogen produced by the burning sodium azide obeys the perfect gas law as it fills the airbag but may have to be modeled as a van der Waal’s gas at the high pressures and temperatures produced in the propellant chamber. The chemical reaction rate law is pressure, particle geometry and surface area dependant, as are most high-pressure burn processes. When the temperature profile of the reacting system is well known, temperature dependent Arrhenius chemical kinetics can be used. Since the airbag propellant composition and performance data are company private information, it is very difficult to obtain the required information for burn rate modeling. However, Imperial Chemical Industries (ICI) Corporation supplied pressure LS-DYNA Theory Manual Equation of State Models exponent, particle geometry, packing density, heat of reaction, and atmospheric pressure burn rate data which allowed us to develop the numerical model presented here for their NaN3 + Fe2O3 driver airbag propellant. The deflagration model, its implementation, and the results for the ICI propellant are presented in the are described by [Hallquist, et. al., 1990]. The unreacted propellant and the reaction product equations-of-state are both of the form: 𝑝 = 𝐴 𝑒−𝑅1𝑉 + 𝐵𝑒−𝑅2𝑉 + 𝜔𝐶v𝑇 𝑉 − 𝑑 , (23.10.24) where 𝑝 is pressure (in Mbars), 𝑉 is the relative specific volume (inverse of relative density), 𝜔 is the Gruneisen coefficient, 𝐶v is heat capacity (in Mbars -cc/cc°K), 𝑇 is temperature in °𝐾, 𝑑 is the co-volume, and 𝐴, 𝐵, 𝑅1 and 𝑅2 are constants. Setting 𝐴 = 𝐵 = 0 yields the van der Waal’s co-volume equation-of-state. The JWL equation-of-state is generally useful at pressures above several kilobars, while the van der Waal’s is useful at pressures below that range and above the range for which the perfect gas law holds. Of course, setting 𝐴 = 𝐵 = 𝑑 = 0 yields the perfect gas law. If accurate values of 𝜔 and 𝐶v plus the correct distribution between “cold” compression and internal energies are used, the calculated temperatures are very reasonable and thus can be used to check propellant performance. The reaction rate used for the propellant deflagration process is of the form: = 𝑍(1 − 𝐹)𝑦 𝐹𝑥 𝑝𝑤 + 𝑉(1 − 𝐹)𝑢 𝐹𝑟𝑝𝑠 ∂𝐹 ∂𝑡 for 0 < 𝐹 < 𝐹limit1 for 𝐹limit2 < 𝐹 < 1 (23.10.25) where 𝐹 is the fraction reacted (𝐹 = 0 implies no reaction, 𝐹 = 1 is complete reaction), 𝑡 is time, and 𝑝 is pressure (in Mbars), 𝑟, 𝑠, 𝑢, 𝑤, 𝑥, 𝑦, 𝐹limit1 and 𝐹limit2 are constants used to describe the pressure dependence and surface area dependence of the reaction rates. Two (or more) pressure dependent reaction rates are included in case the propellant is a mixture or exhibited a sharp change in reaction rate at some pressure or temperature. Burning surface area dependences can be approximated using the (1 − 𝐹)𝑦𝐹𝑥 terms. Other forms of the reaction rate law, such as Arrhenius temperature dependent 𝑒−𝐸/𝑅𝑇 type rates, can be used, but these require very accurate temperatures calculations. Although the theoretical justification of pressure dependent burn rates at kilobar type pressures is not complete, a vast amount of experimental burn rate versus pressure data does demonstrate this effect and hydrodynamic calculations using pressure dependent burn accurately simulate such experiments. The deflagration reactive flow model is activated by any pressure or particle velocity increase on one or more zone boundaries in the reactive material. Such an increase creates pressure in those zones and the decomposition begins. If the pressure is relieved, the reaction rate decreases and can go to zero. This feature is important for Equation of State Models LS-DYNA Theory Manual short duration, partial decomposition reactions. If the pressure is maintained, the fraction reacted eventually reaches one and the material is completely converted to product molecules. The deflagration front rates of advance through the propellant calculated by this model for several propellants are quite close to the experimentally observed burn rate versus pressure curves. To obtain good agreement with experimental deflagration data, the model requires an accurate description of the unreacted propellant equation-of-state, either an analytical fit to experimental compression data or an estimated fit based on previous experience with similar materials. This is also true for the reaction products equation- of-state. The more experimental burn rate, pressure production and energy delivery data available, the better the form and constants in the reaction rate equation can be determined. Therefore the equations used in the burn subroutine for the pressure in the unreacted propellant 𝑃𝑢 = 𝑅1 ⋅ 𝑒−𝑅5⋅𝑉𝑢 + 𝑅2 ⋅ 𝑒−𝑅6⋅𝑉𝑢 + 𝑅3 ⋅ 𝑇𝑢 𝑉𝑢 − FRER , (23.10.26) where 𝑉𝑢 and 𝑇𝑢 are the relative volume and temperature respectively of the unreacted propellant. The relative density is obviously the inverse of the relative volume. The pressure 𝑃p in the reaction products is given by: 𝑃p = 𝐴 ⋅ 𝑒−𝑋𝑃1⋅𝑉𝑝 + 𝐵 ⋅ 𝑒−𝑋𝑃2⋅𝑉𝑝 + 𝐺 ⋅ 𝑇𝑝 𝑉𝑝 − CCRIT . (23.10.27) As the reaction proceeds, the unreacted and product pressures and temperatures are assumed to be equilibrated (𝑇𝑢 = 𝑇𝑝 = 𝑇, 𝑝 = 𝑃𝑢 = 𝑃𝑝) and the relative volumes are additive: 𝑉 = (1 − 𝐹) ⋅ 𝑉𝑢 + 𝐹 ⋅ 𝑉𝑝 (23.10.28) where 𝑉 is the total relative volume. Other mixture assumptions can and have been used in different versions of DYNA2D/3D. The reaction rate law has the form: = GROW1(𝑝 + FREQ)𝑒𝑚(𝐹 + FMXIG)𝑎𝑟1(1 − 𝐹 + FMXIG)𝑒𝑠1 ∂𝐹 ∂𝑡 +GROW2(𝑝 + FREQ)𝑒𝑛(𝐹 + FMXIG) (23.10.29) If 𝐹 exceeds FMXGR, the GROW1 term is set equal to zero, and, if 𝐹 is less thanFMNGR, the GROW2 term is zero. Thus, two separate (or overlapping) burn rates can be used to describe the rate at which the propellant decomposes. This equation-of-state subroutine is used together with a material model to describe the propellant. In the airbag propellant case, a null material model (type #10) can be used. Material type #10 is usually used for a solid propellant or explosive when the shear modulus and yield strength are defined. The propellant material is defined by LS-DYNA Theory Manual Equation of State Models the material model and the unreacted equation-of-state until the reaction begins. The calculated mixture states are used until the reaction is complete and then the reaction product equation-of-state is used. The heat of reaction, ENQ, is assumed to be a constant and the same at all values of 𝐹 but more complex energy release laws could be implemented. LS-DYNA Theory Manual Artificial Bulk Viscosity 24 Artificial Bulk Viscosity Bulk viscosity is used to treat shock waves. Proposed in one spatial dimension by von Neumann and Richtmyer [1950], the bulk viscosity method is now used in nearly all wave propagation codes. A viscous term 𝑞 is added to the pressure to smear the shock discontinuities into rapidly varying but continuous transition regions. With this method the solution is unperturbed away from a shock, the Hugoniot jump conditions remain valid across the shock transition, and shocks are treated automatically. In our discussion of bulk viscosity we draw heavily on works by Richtmyer and Morton [1967], Noh [1976], and Wilkins [1980]. The following discussion of the bulk viscosity applies to solid elements since strong shocks are not normally encountered in structures modeled with shell and beam elements. 24.1 Shock Waves Shock waves result from the property that sound speed increases with increasing pressure. A smooth pressure wave can gradually steepen until it propagates as a discontinuous disturbance called a shock. See Figure 24.1. Shocks lead to jumps in pressure, density, particle velocity, and energy. Consider a planar shock front moving through a material. The velocity ahead of the shock is 𝑢1; the velocity behind is 𝑢2; and the shock velocity is 𝑢𝑠. Mass, momentum, and energy are conserved across the front. Application of these conservation laws leads to the well-known Rankine-Hugoniot jump conditions (𝜌2 − 𝜌1)𝑢𝑠 = 𝜌2𝑢2 − 𝜌1𝑢1 𝜌2(𝑢𝑠 − 𝑢2)𝑢2 + 𝜌1(𝑢1 − 𝑢𝑠)𝑢1 = 𝑝2 − 𝑝1 (𝐸2 − 𝐸1)𝑢𝑠 = (𝐸2 + 𝑝2)𝑢2 − (𝐸1 + 𝑝1)𝑢1 (24.1) (24.2) (24.3) where Equation (24.3) is an expression of the energy jump condition using the results of mass conservation, Equation (24.1), and momentum conservation, Equation (24.2). Artificial Bulk Viscosity LS-DYNA Theory Manual Figure 24.1. If the sound speed increases as the stress increases the traveling wave above will gradually steepen as it moves along the x-coordinate to form a shock wave. Here, 𝜌𝑖 is the density, 𝐸𝑖 is the energy density, and 𝑝𝑖 is the pressure; the subscript, 𝑖, is 1 for ahead of the shock and 2 for behind the shock. The energy equation relating the thermodynamic quantities density, pressure, and energy must be satisfied for all shocks. The equation of state 𝑝 = 𝑝(𝜌, 𝑒), (24.4) which defines all equilibrium states that can exist in a material and relating the same quantities as the energy equation, must also be satisfied. We may use this equation to eliminate energy from Equation (24.3) and obtain a unique relationship between pressure and compression. This relation, called the Hugoniot, determines all pressure- compression states achievable behind the shock. Shocking takes place along the Rayleigh line and not the Hugoniot (Figure 24.1) and because the Hugoniot curve closely approximates an isentrope, we may often assume the unloading follows the Hugoniot. Combining Equations (24.1) and (24.2) and choosing a coordinate fram such that 𝑢1 = 0, we see that the slope of the Rayleigh line is related to the shock speed: 𝑢𝑠 = 𝜌1 √𝑝2 − 𝑝1 √√ − 1 𝜌2 𝜌1 ⎷ . For the material of Figure 24.2, increasing pressure increases shock speed. Consider a 𝛾-law gas with the equation of state 𝑝 = (𝛾 − 1)𝜌𝑒, (24.5) (24.6) LS-DYNA Theory Manual Artificial Bulk Viscosity p1 p0 Figure 24.2. Shocking takes place along the Rayleigh line, and release closely follows the Hugoniot. The cross-hatched area is the difference between the internal energy behind the shock and the internal energy lost on release. where 𝛾 is the ratio of specific heats. Using the energy jump condition, we can eliminate 𝑒 and obtain the Hugoniot 𝑝0 = 𝑝∗ = 2𝑉0 + (𝛾 − 1)(𝑉0 − 𝑉) 2𝑉 − (𝛾 − 1)(𝑉0 − 𝑉) , (24.7) where 𝑉 is the relative volume. Figure 24.3 shows a plot of the Hugoniot and adiabat where it is noted that for 𝑝∗ = 1, the slopes are equal. Thus for weak shocks, Hugoniot and adiabat agree to the first order and can be ignored in numerical calculations. However, special treatment is required for strong shocks, and in numerical calculations this special treatment takes the form of bulk viscosity. 24.2 Bulk Viscosity In the presence of shocks, the governing partial differential equations can give multiple weak solutions. In their discussion of the Rankine-Hugoniot jump conditions, Richtmyer and Morton [1967] report that the unmodified finite difference (element) equations often will not produce even approximately correct answers. One possible solution is to employ shock fitting techniques and treat the shocks as interior boundary conditions. This technique has been used in one spatial dimension but is too complex to extend to multi-dimensional problems of arbitrary geometry. For these reasons the pseudo-viscosity method was a major breakthrough for computational mechanics. Artificial Bulk Viscosity LS-DYNA Theory Manual Limiting compression Hugoniot Adiabat Slopes of Hugoniot and adiabat are equat at Figure 24.3. Hugoniot curve and adiabat for a g-law gas (from [Noh 1976]). The viscosity proposed by von Neumann and Richtmyer [1950] in one spatial dimension has the form 𝑞 = 𝐶0𝜌(Δ𝑥)2 ( ) ∂𝑥̇ ∂𝑥 𝑞 = 0 if if ∂𝑥̇ ∂𝑥 ∂𝑥̇ ∂𝑥 < 0 ≥ 0 (24.8) where 𝐶0 is a dimensionless constant and 𝑞 is added to the pressure in both the momentum and energy equations. When 𝑞 is used, they proved the following for steady state shocks: the hydrodynamic equations possess solutions without discontinuities; the shock thickness is independent of shock strength and of the same order as the Δ𝑥 used in the calculations; the q term is insignificant outside the shock layer; and the jump conditions are satisfied. According to Noh, it is generally believed that these properties: “hold for all shocks, and this has been borne out over the years by countless numerical experiments in which excellent agreement has been obtained either with exact solutions or with hydrodynamical experiments.” In 1955, Landshoff [1955] suggested the addition of a linear term to the 𝑞 of von Neumann and Richtmyer leading to a 𝑞 of the form 𝑞 = 𝐶0𝜌(Δ𝑥)2 ( 𝑞 = 𝐶0𝜌(Δ𝑥)2 ( ) ) 𝜕𝑥̇ 𝜕𝑥 ∂ẋ ∂x − 𝐶1𝜌𝑎Δ𝑥 + 𝐶1𝜌𝑎Δ𝑥 𝜕𝑥̇ 𝜕𝑥 𝜕𝑥̇ 𝜕𝑥 if if 𝜕𝑥̇ 𝜕𝑥 𝜕𝑥̇ 𝜕𝑥 < 0 ≥ 0, (24.9) where 𝐶1 is a dimensionless constant and 𝑎 is the local sound speed. The linear term rapidly damps numerical oscillations behind the shock front (Figure 24.3). A similar form was proposed independently by Noh about the same time. LS-DYNA Theory Manual Artificial Bulk Viscosity In an interesting aside, Wilkins [1980] discusses work by Kuropatenko who, given an equation of state, derived a q by solving the jump conditions for pressure in terms of a change in the particle velocity, Δ𝑢. For an equation of state of the form, 𝑝 = 𝐾 (− 𝜌0 − 1), pressure across the shock front is given by [Wilkins 1980] 𝑝 = 𝑝0 + 𝜌0 (Δ𝑢)2 + 𝜌0|Δ𝑢| [ 2⁄ + 𝑎 2] , (Δ𝑢)2 where 𝑎 is a sound speed 𝑎 = ( 2⁄ . 𝜌0 ) For a strong shock, Δ𝑢2 >> 𝑎2, we obtain the quadratic form and for a weak shock, Δ𝑢2 << 𝑎2, the linear form 𝑞 = 𝜌0Δ𝑢2, 𝑞 = 𝜌0𝑎Δ𝑢, (24.10) (24.11) (24.12) (24.13) (24.14) Thus linear and quadratic forms for 𝑞 can be naturally derived. According to Wilkins, the particular expressions for 𝑞 obtained by Kuropatenko offer no particular advantage over the expressions currently used in most computer programs. In extending the one-dimensional viscosity formulations to multi-dimensions, most code developers have simply replaced the divergence of the velocity with, 𝜀̇𝑘𝑘, the trace of the strain rate tensor, and the characteristic length with the square root of the area A, in two dimensions and the cubic root of the volume v in three dimensions. These changes also give the default viscosities in the LS-DYNA codes: 𝑞 = 𝜌 𝑙(𝐶0𝑙𝜀̇𝑘𝑘 𝑞 = 0 2 − 𝐶𝑙𝑎𝜀̇𝑘𝑘) if 𝜀̇𝑘𝑘 < 0 if 𝜀̇𝑘𝑘 ≥ 0 (24.15) where 𝐶0 and 𝐶1 are dimensionless constants which default to 1.5 and 0.06, respectively, where 1 = √𝐴 in 2D, and √𝑣3 in 3D, a is the local sound speed, 𝐶0 defaults to 1.5 and 𝐶1 defaults to 0.06. In converging two- and three-dimensional geometries, the strain rate 𝜀̇𝑘𝑘 is negative and the 𝑞 term in Equation (24.15) is nonzero, even though no shocks may be generated. This results in nonphysical 𝑞 heating. When the aspect ratios of the elements are poor (far from unity), the use of a characteristic length based on √𝐴 or √𝑣3 can also result in nonphysical 𝑞 heating and even occasional numerical instabilities. Wilkins uses a bulk viscosity that is based in part on earlier work by Richards [1965] Artificial Bulk Viscosity LS-DYNA Theory Manual that extends the von Neumann and Richtmyer formulations in a way that avoids these problems. This latter 𝑞 may be added in the future if the need arises. Wilkins’ 𝑞 is defined as: 𝑞 = 𝐶0𝜌𝑙2 ( ) 𝑑𝑠 𝑑𝑡 − 𝐶𝑙𝜌𝑙𝑎∗ 𝑑𝑠 𝑑𝑡 𝑞 = 0 if 𝜀̇𝑘𝑘 < 0 if 𝑑𝑠 𝑑𝑡 ≥ 0 (24.16) where 𝑙 and 𝑑𝑠 𝑑𝑡 are the thickness of the element and the strain rate in the direction of the acceleration, respectively, and 𝑎∗ is the sound speed defined by (p/𝜌)1/2 if 𝑝 > 0. We use the local sound speed in place of 𝑎∗ to reduce the noise at the low stress levels that are typical of our applications. Two disadvantages are associated with Equation (24.16). To compute the length parameter and the strain rate, we need to know the direction of the acceleration through the element. Since the nodal force vector becomes the acceleration vector in the explicit integration scheme, we have to provide extra storage to save the direction. In three dimensions our present storage capacity is marginal at best and sacrificing this storage for storing the direction would make it even more so. Secondly, we need to compute l and 𝑑𝑠 𝑑𝑡 which results in a noticeable increase in computer cost even in two dimensions. For most problems the additional refinement of Wilkins is not needed. However, users must be aware of the pitfalls of Equation (24.15), i.e., when the element aspect ratios are poor or the deformations are large, an anomalous 𝑞 may be generated. LS-DYNA Theory Manual Time Step Control 25 Time Step Control During the solution we loop through the elements to update the stresses and the right hand side force vector. We also determine a new time step size by taking the minimum value over all elements. Δ𝑡𝑛+1 = 𝑎 ⋅ min{Δ𝑡1, Δ𝑡2, Δ𝑡3, . . . , Δ𝑡𝑁}, (25.1) where 𝑁 is the number of elements. For stability reasons the scale factor 𝑎 is typically set to a value of .90 (default) or some smaller value. 25.1 Time Step Calculations for Solid Elements A critical time step size, Δ𝑡𝑒, is computed for solid elements from Δ𝑡𝑒 = 𝐿𝑒 {[𝑄 + (𝑄2 + 𝑐2)1/2]} where 𝑄 is a function of the bulk viscosity coefficients 𝐶0 and 𝐶1: 𝑄 = { 𝐶1𝑐 + 𝐶0𝐿𝑒|𝜀̇𝑘𝑘| for 𝜀̇𝑘𝑘 ≤ 0 for 𝜀̇𝑘𝑘 > 0 (25.2) (25.3) 𝐿𝑒 is a characteristic length: 8 node solids: 𝐿𝑒 = 4 node tetrahedras: 𝐿𝑒 = minimum altitude 𝜐𝑒 𝐴𝑒max 𝜐𝑒 is the element volume, 𝐴𝑒max is the area of the largest side, and 𝑐 is the adiabatic sound speed: 𝑐 = [ 4𝐺 3𝜌0 + ∂𝑝 ∂𝜌 ) 2⁄ ] , (25.4) where 𝜌 is the specific mass density. Noting that: Time Step Control LS-DYNA Theory Manual ∂𝑝 ∂𝜌 ) = ∂𝑝 ∂𝜌 ) + ∂𝑝 ∂𝑈 ) ∂𝑈 ∂𝜌 , ) (25.5) and that along an isentrope the incremental energy, 𝑈, in the units of pressure is the product of pressure, 𝑝, and the incremental relative volume, 𝑑𝑉: we obtain 𝑑𝑈 = −𝑝𝑑𝑉, 𝑐 = ⎡ 4𝐺 ⎢ 3𝜌0 ⎣ + ∂𝑝 ∂𝜌 ) + 𝑝𝑉2 𝜌0 ∂𝑝 ∂𝑈 ) 2⁄ ⎤ ⎥ 𝜌⎦ . (25.6) (25.7) For elastic materials with a constant bulk modulus the sound speed is given by: 𝑐 = √ 𝐸(1 − 𝜐) (1 + 𝜐)(1 − 2𝜐)𝜌 (25.8) where 𝐸 is Young’s modulus, and 𝜐 is Poisson’s ratio. 25.2 Time Step Calculations for Beam and Truss Elements For the Hughes-Liu beam and truss elements, the time step size is given by: where 𝐿 is the length of the element and c is the wave speed: Δ𝑡𝑒 = 𝑐 = √ . (25.9) (25.10) For the Belytschko beam the time step size given by the longitudinal sound speed is used (Equation (25.9)), unless the bending-related time step size given by [Belytschko and Tsay 1982] Δ𝑡𝑒 = 𝑐√3𝐼 [ 0.5𝐿 12𝐼 + 𝐴𝐿2 + 1 𝐴𝐿2] (25.11) is smaller, where 𝐼 and 𝐴 are the maximum value of the moment of inertia and area of the cross section, respectively. Comparison of critical time steps of the truss versus the elastic solid element shows that it if Poisson's ratio, 𝜐, is nonzero the solid elements give a considerably smaller stable time step size. If we define the ratio, 𝛼, as: LS-DYNA Theory Manual Time Step Control 𝛼 = Δ𝑡continuum Δ𝑡rod = 𝐶rod 𝐶continuum = √ (1 + 𝜐)(1 − 2𝜐) , 1 − 𝜐 (25.12) we obtain the results in Table 22.1 where we can see that as υ approaches .5 𝛼 → 0. 0 1. 0.2 0.949 0.3 0.862 0.4 0.683 0.45 0.513 0.49 0.242 0.50 0.0 Table 22.1. Comparison of critical time step sizes for a truss versus a solid element. 25.3 Time Step Calculations for Shell Elements For the shell elements, the time step size is given by: where 𝐿𝑠 is the characteristic length and 𝑐 is the sound speed: Δ𝑡𝑒 = 𝐿𝑠 𝑐 = √ 𝜌(1 − 𝜈2) . (25.13) (25.14) Three user options exists for choosing the characteristic length. In the default or first option the characteristic length is given by: 𝐿𝑠 = (1 + 𝛽)𝐴𝑠 max(𝐿1, 𝐿2, 𝐿3, (1 − 𝛽)𝐿4) (25.15) where 𝛽 = 0 for quadrilateral and 1 for triangular shell elements, 𝐴𝑠 is the area, and 𝐿𝑖, (𝑖 = 1. . . .4) is the length of the sides defining the shell elements. In the second option a more conservative value of 𝐿𝑠 is used: (1 + 𝛽)𝐴𝑠 , max(𝐷1, 𝐷2) 𝐿𝑠 = (25.16) where 𝐷𝑖(𝑖 = 1,2) is the length of the diagonals. The third option provides the largest time step size and is frequently used when triangular shell elements have very short altitudes. The bar wave speed, Equation (21.10), is used to compute the time step size and 𝐿𝑠 is given by 𝐿𝑠 = max [ (1 + 𝛽)𝐴𝑠 max(𝐿1, 𝐿2, 𝐿3, (1 − 𝛽)𝐿4) , min(𝐿1, 𝐿2, 𝐿3, 𝐿4 + 𝛽1020)]. (25.17) A comparison of critical time steps of truss versus shells is given in Table 22.2 with 𝛽 defined as: Time Step Control LS-DYNA Theory Manual 𝛽 = Δ𝑡2D-continuum Δ𝑡rod = 𝐶rod = √1 − 𝜐2. (25.18) 0 1.0 0.2 0.98 0.3 0.954 0.4 0.917 0.5 0.866 Table 22.2. Comparison of critical time step sizes for a truss versus a shell element. 25.4 Time Step Calculations for Solid Shell Elements A critical time step size, Δ𝑡𝑒 is computed for solid shell elements from 𝜐𝑒 𝑐𝐴𝑒max where 𝜐𝑒 is the element volume, 𝐴𝑒max is the area of the largest side, and 𝑐 is the plane stress sound speed given in Equation (25.14). Δ𝑡𝑒 = (25.19) , 25.5 Time Step Calculations for Discrete Elements For spring elements such as that in Figure 25.1 there is no wave propagation speed 𝑐 to calculate the critical time step size. The eigenvalue problem for the free vibration of spring with nodal masses 𝑚1 and 𝑚2, and stiffness, 𝑘, is given by: [ 𝑘 −𝑘 −𝑘 ] [ 𝑢1 𝑢2 ] − 𝜔2 [ 𝑚1 𝑚2 ] [ 𝑢1 𝑢2 ] = [0 ]. (25.20) Since the determinant of the characteristic equation must equal zero, we can solve for the maximum eigenvalue: det [ 𝑘 − 𝜔2𝑚1 −𝑘 −𝑘 𝑘 − 𝜔2𝑚2 ] = 0 → 𝜔max 2 = 𝑘(𝑚1 + 𝑚2) 𝑚1 ⋅ 𝑚2 , (25.21) LS-DYNA Theory Manual Time Step Control m1 = 0.5M1 ; M1 = nodal mass m2 = 0.5M2 ; M2 = nodal mass Figure 25.1. Lumped spring mass system. Recalling the critical time step of a truss element: Δ𝑡 ≤ 𝜔max = ⎫ }} ⎬ 2𝑐 }} ℓ ⎭ Δ𝑡 ≤ 𝜔max , (25.22) and approximating the spring masses by using 1/2 the actual nodal mass, we obtain: Δ𝑡 = 2√ 𝑚1𝑚2 𝑚1 + 𝑚2 . (25.23) Therefore, in terms of the nodal mass we can write the critical time step size as: Δ𝑡𝑒 = √ 2𝑀1𝑀2 𝑘(𝑀1 + 𝑀2) . (25.24) The springs used in the contact interface are not checked for stability. LS-DYNA Theory Manual Boundary and Loading Conditions 26 Boundary and Loading Conditions 26.1 Pressure Boundary Conditions Consider pressure loadings on boundary ∂b1 in Equation (2.4). To carry out the surface integration indicated by the integral a Gaussian quadrature rule is used. To locate any point of the surface under consideration, a position vector, 𝑟, is defined: ∫ 𝑁𝑡𝑡𝑑𝑠 ∂𝑏1 , (26.1) where 𝑟 = 𝑓1(𝜉 , 𝜂)𝑖1 + 𝑓2((𝜉 , 𝜂)𝑖2 + 𝑓3(𝜉 , 𝜂)𝑖3, 𝑓𝑖(𝜉 , 𝜂) = ∑ 𝜙𝑗𝑥𝑖 , 𝑗=1 (26.2) (26.3) and 𝑖1, 𝑖2, 𝑖3 are unit vectors in the 𝑥1, 𝑥2, 𝑥3directions . Nodal quantities are interpolated over the four-node linear surface by the functions 𝜙𝑖 = (1 + 𝜉 𝜉𝑖)(1 + 𝜂𝜂𝑖), (26.4) so that the differential surface area 𝑑𝑠 may be written in terms of the curvilinear coordinates as where |𝐽| is the surface Jacobian defined by 𝑑𝑠 = |𝐽|𝑑𝜉𝑑𝜂, |𝐽| = ∣ ∂𝑟 ∂𝜉 × ∂𝑟 ∂𝜂 2⁄ ∣ = (𝐸𝐺 − 𝐹2) , (26.5) (26.6) in which Boundary and Loading Conditions LS-DYNA Theory Manual x3 i3 i2 r(ξ,η) x1 x2 i1 Figure 26.1. Parametric representation of a surface segment. 𝐸 = 𝐹 = 𝐺 = ∂𝑟 ∂𝜉 ∂𝑟 ∂𝜉 ∂𝑟 ∂𝜂 ⋅ ⋅ ⋅ ∂𝑟 ∂𝜉 ∂𝑟 ∂𝜂 ∂𝑟 ∂𝜂 , , . A unit normal vector 𝐧 to the surface segment is given by 𝐧 = |𝐽| −1 ( ∂𝐫 ∂𝜉 × ∂𝐫 ∂𝜂 ), and the global components of the traction vector can now be written 𝑡𝑖 = 𝑛𝑖 ∑ 𝜙𝑗𝑝𝑗 𝑗=1 , where 𝑝𝑗 is the applied pressure at the jth node. The surface integral for a segment is evaluated as: (26.7) (26.8) (26.9) ∫ ∫ 𝑁𝑡𝑡|𝐽|𝑑𝜉 𝑑𝜂 −1 −1 . (26.10) One such integral is computed for each surface segment on which a pressure loading acts. Note that the Jacobians cancel when Equations (26.8) and (26.7) are put into Equation (26.10). Equation (26.10) is evaluated with one-point integration analogous to that employed in the volume integrals. The area of an element side is approximated by 4|𝐽| where |𝐽| = |𝐽(0, 0)|. LS-DYNA Theory Manual Boundary and Loading Conditions 26.2 Transmitting Boundaries Transmitting boundaries are available only for problems that require the modeling of semi-infinite or infinite domains with solid elements and therefore are not available for beam or shell elements. Applications of this capability include problems in geomechanics and underwater structures. The transmitting or silent boundary is defined by providing a complete list of boundary segments. In the approach used, discussed by Cohen and Jennings [1983] who in turn credit the method to Lysmer and Kuhlemeyer [1969], viscous normal shear stresses in Equation (23.11) are applied to the boundary segments: 𝛔normal = −𝜌𝑐𝑑𝐕normal 𝛔shear = −𝜌𝑐𝑠𝐕tan, (26.11) (26.12) where 𝜌, 𝑐𝑑,and 𝑐𝑠 are the material density, dilatational wave speed, and the shear wave speed of the transmitting media respectively. The magnitude of these stresses is proportional to the particle velocities in the normal, 𝐕normal, and tangential, 𝐕tan, directions. The material associated with each transmitting segment is identified during initialization so that unique values of the constants 𝜌, 𝑐𝑑, and 𝑐𝑠 can be defined automatically. 26.3 Kinematic Boundary Conditions In this subsection, the kinematic constraints are briefly reviewed. LS-DYNA tracks reaction forces for each type of kinematic constraint and provides this information as output if requested. For the prescribed boundary conditions, the input energy is integrated and included in the external work. 26.4 Displacement Constraints Translational and rotational boundary constraints are imposed either globally or locally by setting the constrained acceleration components to zero. If nodal single point constraints are employed, the constraints are imposed in a local system. The user defines the local system by specifying a vector 𝐮1 in the direction of the local x-axis 𝐱l, and a local in-plane vector 𝐯l. After normalizing 𝐮1, the local 𝐱𝑙, 𝐲𝑙and 𝐳l axes are given by: Boundary and Loading Conditions LS-DYNA Theory Manual 𝐱𝑙 = 𝐮𝑙 ‖𝐮𝑙‖ 𝐳𝑙 = 𝐱𝑙 × 𝐯𝑙 ‖𝐱𝑙 × 𝐯𝑙‖ 𝐲𝑙 = 𝐳𝑙 × 𝐱𝑙. (26.13) (26.14) (26.15) A transformation matrix 𝐪 is constructed to transform the acceleration components to the local system: 𝐪 = 𝐱𝑙 ⎤ ⎡ ⎥⎥ ⎢⎢ , 𝐲𝑙 T ⎦ 𝐳𝑙 ⎣ (26.16) and the nodal translational and rotational acceleration vectors 𝐚𝐼 and 𝛚̇ 𝐼, for node I are transformed to the local system: 𝐚𝐼1 = 𝐪𝐚𝐼 𝛚̇ 𝐼𝑙 = 𝐪𝛚̇ 𝐼, (26.17) (26.18) and the constrained components are zeroed. transformed back to the global system: The modified vectors are then 𝐚𝐼 = 𝐪T𝐚𝐼1 𝛚̇ 𝐼 = 𝐪T𝛚̇ 𝐼𝑙 (26.19) (26.20) 26.5 Prescribed Displacements, Velocities, and Accelerations Prescribed displacements, velocities, and accelerations are treated in a nearly identical way to displacement constraints. After imposing the zero displacement constraints, the prescribed values are imposed as velocities at time, 𝑡𝑛+1/2. The acceleration versus time curve is integrated or the displacement versus time curve is differentiated to generate the velocity versus time curve. The prescribed nodal components are then set. LS-DYNA Theory Manual Boundary and Loading Conditions 26.6 Body Force Loads Body force loads are used in many applications. For example, in structural analysis the base accelerations can be applied in the simulation of earthquake loadings, the gun firing of projectiles, and gravitational loads. The latter is often used with dynamic relaxation to initialize the internal forces before proceeding with the transient response calculation. In aircraft engine design the body forces are generated by the application of an angular velocity of the spinning structure. The generalized body force loads are available if only part of the structure is subjected to such loadings, e.g., a bird striking a spinning fan blade. For base accelerations and gravity we can fix the base and apply the loading as part of the body force loads element by element according to Equation (22.18) 𝐟𝑒body = ∫ 𝜌𝐍T𝐍𝐚base𝑑𝜐 𝜐𝑚 = 𝐦𝑒𝐚base, (26.21) where 𝐚base is the base acceleration and 𝐦𝑒 is the element (lumped) mass matrix. LS-DYNA Theory Manual Time Integration 27 Time Integration 27.1 Background Consider the single degree of freedom damped system in Figure 27.1. p(t) u(t) - displacements Figure 27.1. Single degree of freedom damped system. Forces acting on mass m are shown in Figure 27.2. The equations of equilibrium are obtained from d'Alembert’s principle 𝑓𝐼 + 𝑓𝐷 + 𝑓int = 𝑝(𝑡) (27.1) fI inertia force p(t) external forces elastic force fs fD damping forces Figure 27.2. Forces acting on mass, m Time Integration LS-DYNA Theory Manual 𝑓𝐼 = 𝑚𝑢̈; 𝑢̈ = 𝑓𝐷 = 𝑐𝑢̇; 𝑢̇ = 𝑓int = 𝑘 ⋅ 𝑢; 𝑑2𝑢 𝑑𝑡2 acceleration 𝑑𝑢 velocity 𝑑𝑡 𝑢 displacement (27.2) where 𝑐 is the damping coefficient, and k is the linear stiffness. For critical damping 𝑐 = ccr. The equations of motion for linear behavior lead to a linear ordinary differential equation, o.d.e.: 𝑚𝑢̈ + 𝑐𝑢̇ + 𝑘𝑢 = 𝑝(𝑡) (27.3) but for the nonlinear case the internal force varies as a nonlinear function of the displacement, leading to a nonlinear o.d.e.: 𝑚𝑢̈ + 𝑐𝑢̇ + 𝑓int(𝑢) = 𝑝(𝑡) (27.4) Analytical solutions of linear ordinary differential equations are available, so instead we consider the dynamic response of linear system subjected to a harmonic loading. It is convenient to define some commonly used terms: Harmonic loading: 𝑝(𝑡) = 𝑝0sin𝜛𝑡 Circular frequency: 𝜔 = √ 𝑘 2𝜋 = 1 Natural frequency: 𝑓 = 𝜔 = 𝑐 𝜉 = 𝑐 Damping ratio: 𝑐𝑐𝑟 𝑇 𝑇 = period 2𝑚𝜔 𝑚 for single degree of freedom Damped vibration frequency: Applied load frequency: 𝛽 = 𝜔̅̅̅̅̅ 𝜔 𝜔0 = 𝜔√1 − 𝜉 2 The closed form solution is: 𝑢̇0 𝑝0 sin𝜔𝑡 + 𝑢(𝑡) = 𝑢0cos𝜔𝑡 + 1 − 𝛽2 (sin𝜔̅̅̅̅𝑡 − 𝛽sin𝜔𝑡) homogeneous solution steady state transient particular solution (27.5) with the initial conditions: 𝑢0 = initial displacement 𝑢̇0 = initial velocity 𝑝0 = static displacement For nonlinear problems, only numerical solutions are possible. LS-DYNA uses the explicit central difference scheme to integrate the equations of motion. LS-DYNA Theory Manual Time Integration 27.2 The Central Difference Method The semi-discrete equations of motion at time n are: (27.6) where 𝐌 is the diagonal mass matrix, 𝐏𝑛 accounts for external and body force loads, 𝑭 𝑛 is the stress divergence vector, and 𝐇𝑛 is the hourglass resistance. To advance to time 𝑡𝑛+1, we use central difference time integration: 𝐌𝐚𝑛 = 𝐏𝑛 − 𝐅𝑛 + 𝐇𝑛, 𝐚𝑛 = 𝐌−1(𝐏𝑛 − 𝐅𝑛 + 𝐇𝑛), 𝐯𝑛+1 2⁄ = 𝐯𝑛−1 2⁄ + 𝐚𝑛Δ𝑡𝑛, 𝐮𝑛+1 = 𝐮𝑛 + 𝐯𝑛+1 2⁄ Δ𝑡𝑛+1 2⁄ , (27.7) (27.8) (27.9) where (Δ𝑡𝑛 + Δ𝑡𝑛+1) , and 𝐯 and 𝐮 are the global nodal velocity and displacement vectors, respectively. We update the geometry by adding the displacement increments to the initial geometry: Δ𝑡𝑛+1 2⁄ = (27.10) 𝐱𝑛+1 = 𝐱0 + 𝐮𝑛+1. (27.11) We have found that, although more storage is required to store the displacement vector the results are much less sensitive to round-off error. 27.3 Stability of Central Difference Method The stability of the central difference scheme is determined by looking at the stability of a linear system. The system of linear equations in uncoupled into the modal equations where the modal matrix of eigenvectors, 𝛟, are normalized with respect to the mass and linear stiffness matrices 𝐊, and 𝐌, respectively, such that: 𝛟T𝐌𝛟 = I 𝛟T𝐊𝛟 = ω2. (27.12) With this normalization, we obtain for viscous proportional damping the decoupling of the damping matrix, 𝐂: The equations of motion in the modal coordinates 𝐱 are: 𝛟T𝐂𝛟 = 2𝜉𝜔 𝑥̈ + 2𝜉ω𝑥̇ + ω2𝑥 = 𝛟𝐓𝐩⏟ . =Y (27.13) (27.14) With central differences we obtain for the velocity and acceleration: Time Integration LS-DYNA Theory Manual 𝑥̇𝑛 = 𝑥𝑛+1 − 𝑥𝑛−1 2Δ𝑡 𝑥̈𝑛 = 𝑥𝑛+1 − 2𝑥𝑛 + 𝑥𝑛−1 Δ𝑡2 . Substituting 𝑥̇𝑛 and 𝑥̈𝑛 into equation of motion at time 𝑡𝑛 leads to: 𝑥𝑛+1 = 2 − 𝜔2Δ𝑡2 1 + 2𝜉𝜔Δ𝑡2 𝑥𝑛 − 1 − 2𝜉𝜔Δ𝑡 1 + 2𝜉𝜔Δ𝑡 𝑥𝑛−1 + Δ𝑡2 1 + 2𝜉𝜔Δ𝑡2 𝑌𝑛, which in matrix form leads to 𝑥𝑛 = 𝑥𝑛, [ 𝑥𝑛+1 𝑥𝑛 ] = 2 − 𝜔2Δ𝑡2 1 + 2𝜉𝜔Δ𝑡 ⎡ ⎢ ⎣ − 1 − 2𝜉𝜔Δ𝑡 1 + 2𝜉𝜔Δ𝑡 ⎤ ⎥ ⎦ [ 𝑥𝑛 𝑥𝑛−1 ] + Δ𝑡2 ⎡ ⎢ 1 + 2𝜉𝜔Δ𝑡2 ⎣ ⎤ ⎥ ⎦ 𝑌𝑛, or 𝐱̂𝑛+1 = 𝐀𝐱̂𝑛 + 𝐋𝐘𝑛, (27.15) (27.16) (27.17) (27.18) (27.19) (27.20) where, 𝐀 is the time integration operator for discrete equations of motion. After 𝑚 time steps with 𝐋 = 0 we obtain: As 𝑚 approaches infinity, 𝐀 must remain bounded. 𝐱̂𝑚 = 𝐀𝑚𝐱̂0. A spectral decomposition of 𝐴 gives: 𝐀𝑚 = (𝐏T𝐉𝐏) = 𝐏T𝐉𝑚𝐏, (27.21) (27.22) where, 𝐏, is the orthonormal matrix containing the eigenvectors of 𝐀, and 𝐉 is the Jordan form with the eigenvalues on the diagonal. The spectral radius, 𝜌(𝐀), is the largest eigenvalue of 𝐀 = max [diag. (J)]. We know that 𝐉𝑚, is bounded if and only if: ∣𝜌(𝐀)∣ ≤ 1. Consider the eigenvalues of 𝐴 for the undamped equation of motion Det [∣2 − 𝜔2Δ𝑡2 −1 ∣ − 𝜆∣1 −1 ∣] = 0, −(2 − 𝜔2Δ𝑡2 − 𝜆) ⋅ 𝜆 + 1 = 0, 𝜆 = 2 − 𝜔2Δ𝑡2 ± √ (2 − 𝜔2Δ𝑡2)2 − 1. (27.23) (27.24) (27.25) (27.26) The requirement that |𝜆| ≤ 1 leads to: LS-DYNA Theory Manual Time Integration Δ𝑡 ≤ 𝜔max , as the critical time step. For the damped equations of motion we obtain: Δ𝑡 ≤ 𝜔max (√1 + 𝜉 2 − 𝜉 ). (27.27) (27.28) Thus, damping reduces the critical time step size. The time step size is bounded by the largest natural frequency of the structure which, in turn, is bounded by the highest frequency of any individual element in the finite element mesh. 27.4 Subcycling (Mixed Time Integration) The time step size, Δ𝑡, is always limited by a single element in the finite element mesh. The idea behind subcycling is to sort elements based on their step size into groups whose step size is some even multiple of the smallest element step size, 2(𝑛−1)Δ𝑡, for integer values of 𝑛 greater than or equal to 1. For example, in Figure 27.3 the mesh on the right because of the thin row of elements is three times more expensive than the mesh on the left The subcycling in LS-DYNA is based on the linear nodal interpoation partition subcycling algorithm of Belytschko, Yen, and Mullen [1979], and Belytschko [1980]. In their implementation the steps are: 1. 2. 3. Assign each node, 𝑖, a time step size, Δ𝑡𝑗, according to: Δ𝑡𝑖 = min (2 𝜔𝑗⁄ ) over all elements 𝑗, connected to node 𝑖 Assign each element, 𝑗, a time step size, Δ𝑡𝑗, according to: Δ𝑡𝑗 = min(Δ𝑡𝑖) over all nodes, 𝑖, of element, 𝑗 Group elements into blocks by time step size for vectorization. Figure 27.3. The right hand mesh is much more expensive to compute than the left hand due to the presence of the thinner elements. Time Integration LS-DYNA Theory Manual In LS-DYNA we desire to use constant length vectors as much as possible even if it means updating the large elements incrementally with the small time step size. We have found that doing this decreases costs and stability is unaffected. Hulbert and Hughes [1988] reviewed seven subcycling algorithms in which the partitioning as either node or element based. The major differences within the two subcycling methods lie in how elements along the interface between large and small elements are handled, a subject which is beyond the scope of this theoretical manual. Nevertheless, they concluded that three of the methods including the linear nodal interpolation method chosen for LS-DYNA, provide both stable and accurate solutions for the problems they studied. However, there was some concern about the lack of stability and accuracy proofs for any of these methods when applied to problems in structural mechanics. The implementation of subcycling currently includes the following element classes and contact options: • • • • • Solid elements Beam elements Shell elements Brick shell elements Penalty based contact algorithms. but intentionally excludes discrete elements since these elements generally contribute insignificantly to the calculational costs. The interface stiffnesses used in the contact algorithms are based on the minimum value of the slave node or master segment stiffness and, consequently, the time step size determination for elements on either side of the interface is assumed to be decoupled; thus, scaling penalty values to larger values when subcycling is active can be a dangerous exercise indeed. Nodes that are included in constraint equations, rigid bodies, or in contact with rigid walls are always assigned the smallest time step sizes. To explain the implementation and the functioning of subcycling, we consider the beam shown in Figure 27.4 where the beam elements on the right (material group 2) have a Courant time step size exactly two times greater than the elements on the left. The nodes attached to material group 2 will be called minor cycle nodes and the rest, major cycle nodes. At time step 𝑛 = 𝑚𝑘 all nodal displacements and element stresses are known, where 𝑚 is the ratio between the largest and smallest time step size, 𝑘 is the number of major time steps, and 𝑛 is the number of minor time steps. In Figures 27.5 and 27.6, the update of the state variables to the next major time step 𝑘 + 1 is depicted. The stress state in the element on the material interface in group 1 is updated during the minor cycle as the displacement of the major cycle node shared by this element is assumed to vary linearly during the minor cycle update. This linear variation of the major cycle nodal displacements during the update of the element stresses improves accuracy and stability. LS-DYNA Theory Manual Time Integration Material Group 1 Material Group 2 E2 = 4E1 A2 = A1 2 = ρ 1 F(t) Figure 27.4. Subcycled beam problem from Hulbert and Hughes [1988]. In the timing study results in Table 24.1, fifty solid elements were included in each group for the beam depicted in Figure 27.4, and the ratio between 𝐸2 to 𝐸1 was varied from 1 to 128 giving a major time step size greater than 10 times the minor. Note that as the ratio between the major and minor time step sizes approaches infinity the reduction in cost should approach 50 percent for the subcycled case, and we see that this is indeed the case. The effect of subcycling for the more expensive fully integrated elements is greater as may be expected. The overhead of subcycling for the case where 𝐸1 = 𝐸2 is relatively large. This provides some insight into why a decrease in speed is often observed when subcycling is active. For subcycling to have a significant effect, the ratio of the major to minor time step size should be large and the number of elements having the minor step size should be small. In crashworthiness applications the typical mesh is very well planned and generated to have uniform time step sizes; consequently, subcycling will probably give a net increase in costs. Time Integration LS-DYNA Theory Manual u2 v2 u2 v2 Solve for accelerations, velocities, and displacements Solve for minor cycle stresses u1 v1 u1 v1 Figure 27.5. Timing diagram for subcycling algorithm based on linear nodal interpolations. Case 1 one point integration with elastic material model Number of cycles cpu time(secs) 𝐸2 = 𝐸1 𝐸2 = 4𝐸1 𝐸2 = 16𝐸1 𝐸2 = 64𝐸1 𝐸2 = 128𝐸1 178 178 367 367 714 715 1417 1419 2003 2004 4.65 5.36 (+15.%) 7.57 7.13 (-6.0%) 12.17 10.18 (-20.%) 23.24 16.39 (-29.%) 31.89 22.37 (-30.%) Case 2 eight point integration with orthotropic material model Number of cycles cpu time(secs) LS-DYNA Theory Manual Time Integration u2 v2 u2 v2 u1 v1 Solve for minor cycle accelerations, velocities, and displacements u2 v2 u2 v2 u1 v1 Update stress for all elements Figure 27.6. Timing diagram for subcycling algorithm based on linear nodal interpolations. 𝐸2 = 𝐸1 𝐸2 = 4𝐸1 𝐸2 = 16𝐸1 𝐸2 = 64𝐸1 𝐸2 = 128𝐸1 180 180 369 369 718 719 1424 1424 2034 2028 22.09 22.75 (+3.0%) 42.91 34.20 (-20.%) 81.49 54.75 (-33.%) 159.2 97.04 (-39.%) 226.8 135.5 (-40.%) Table 24.1. Timing study showing effects of the ratio of the major to minor time step size. The impact of the subcycling implementation in the software has a very significant effect on the internal structure. The elements in LS-DYNA are now sorted three times Time Integration LS-DYNA Theory Manual Time Integration Loop update velocities write databases update displacements and new geometry kinematic based contact and rigid walls update accelerations and apply kinematic b.c.'s update current time and check for termination Start apply force boundary conditions process penalty based contact interfaces process brick,beam, shell elements process discrete elements Figure 27.7. The time integration loop in LS-DYNA. By element number in ascending order. By material number for large vector blocks. • • By connectivity to insure disjointness for right hand side vectorization which is • very important for efficiency. Sorting by Δ𝑡, interact with the second and third sorts and can result in the creation of much smaller vector blocks and result in higher cost per element time step. During the simulation elements can continuously change in time step size and resorting may be required to maintain stability; consequently, we must check for this continuously. Sorting cost, though not high when spread over the entire calculation, can become a factor that results in higher overall cost if done too frequently especially if the factor, m, is relatively small and the ratio of small to large elements is large. LS-DYNA Theory Manual Rigid Body Dynamics 28 Rigid Body Dynamics A detailed discussion of the rigid body algorithm is presented by Benson and Hallquist [1986] and readers are referred to this publication for more information. The equations of motion for a rigid body are given by 𝑥, 𝑀𝜌𝒙̈ = 𝒇𝜌 𝑱𝜌𝝎̇ + 𝝎 × 𝑱𝜌𝝎 = 𝒇𝜌 𝜔, (28.1) (28.2) where 𝑀𝜌 is the physical mass, 𝑱𝜌 is the physical inertia tensor, 𝒙 is the location of the 𝜔 are the forces and center of mass, 𝝎 is the angular velocity of the body, and 𝒇𝜌 torques applied to the rigid body through *LOAD_RIGID_BODY. These are equations that can be found in a standard text book on rigid body mechanics. The physical properties of a rigid body may come from three sources, these are 𝑥 and 𝒇𝜌 1.Integration of the mass density 𝜌 over a region 𝑉 occupied by the rigid body, for which 𝑀𝜌 = ∫ 𝜌𝑑𝑉, and 𝑱𝜌 = ∫ 𝜌(𝒚 − 𝒙)⨂(𝒚 − 𝒙)𝑑𝑉. The initial rigid body coordinate 𝒙 is in this case determined from 𝒙 = ∫ 𝜌𝒚𝑑𝑉 𝑀𝜌 . Here 𝒚 is the integrand variable. 2.Specifying properties using *PART_INERTIA, for which 𝑀𝜌, 𝑱𝜌 and initial coordinate 𝒙 is simply specified in the keyword input deck. 3.For a nodal rigid body, *CONSTRAINED_NODAL_RIGID_BODY, the physical properties vanish, i.e., 𝑀𝜌 = 0 and 𝑱𝜌 = 𝟎, and the position is arbitrary. All rigid bodies possess slave nodes, which play a role when rigid bodies in LS-DYNA interact with their surroundings. Slave nodes may come from the following. 1.The nodes in the finite element mesh for the part specified as rigid through *MAT_RIGID. 2.Extra nodes definitions through *CONSTRAINED_EXTRA_NODES. 3.The set used for a nodal rigid body in *CONSTRAINED_NODAL_RIGID_BODY. Rigid Body Dynamics LS-DYNA Theory Manual We use 𝑆 to denote the set of slave nodes to the rigid body, and these are constrained to the rigid body through the equations 𝒙𝑖 = 𝒙 + 𝑸(𝒙𝑖 0 − 𝒙0), 𝑸𝑖 = 𝑸, (28.3) (28.4) for all 𝑖 ∈ 𝑆. Here we have introduced the orientations 𝑸 and 𝑸𝑖 of the rigid body and slave node 𝑖, respectively. Furthermore, 𝒙𝑖 is the coordinate of slave node 𝑖 and we use superscript 0 to denote a quantity at time zero. The time evolution of 𝑸 is 𝑸̇ = 𝜴𝑸, (28.5) where 𝛀𝒓 = 𝝎 × 𝒓 for an arbitrary vector 𝒓 and 𝑸 = 𝑰 (identity) at time zero. So equations (28.3) and (28.4) can equivalently be put in rate form 𝒙̇𝑖 = 𝒙̇ + 𝝎 × 𝒓𝑖, 𝝎𝑖 = 𝝎, (28.6) (28.7) where 𝒓𝑖 = 𝒙𝑖 − 𝒙 and understandably 𝝎𝑖 rotational velocity of slave node 𝑖. This also determines the space of admissible virtual displacement for the slave nodes in the context of work principles, and for this reason we use a compact notation for this equation [ 𝒙̇𝑖 𝝎𝑖 ] = [ 𝑰 −𝑹𝑖 ] [ 𝒙̇ ]. (28.8) where 𝑹𝑖𝒓 = 𝒓𝑖 × 𝒓 for an arbitrary vector 𝒓. Slave nodes may have masses 𝑚𝑖, inertias 𝑱𝑖 and forces 𝒇𝑖 𝑥 and 𝒇𝑖 𝜔 associated with them. The inertia properties may come from 1.Mass contributions from deformable elements connected to the rigid body, either or through *CONSTRAINED_NODAL_RIGID_BODY or simply merged mesh. 2.Lumped masses through *ELEMENT_MASS or *ELEMENT_INERTIA. *CONSTRAINED_EXTRA_NODES and the forces may come from 1.External loads through *LOAD_NODE or *LOAD_SEGMENT. 2.Contacts or fluid structure interaction (FSI) or similar. 3.Internal forces on deformable nodes of a contiguous part. Note that these quantities exclude any contributions from and on the rigid body itself, 𝜔. The motion of the slave nodes is governed as these are all collected in 𝑀𝜌, 𝑱𝜌, 𝒇𝜌 by their own equations of motion 𝑥 and 𝒇𝜌 28-2 (Rigid Body Dynamics) 𝑚𝑖𝒙̈𝑖 = 𝒇𝑖 𝑥, LS-DYNA Theory Manual Rigid Body Dynamics 𝑱𝑖𝝎̇𝑖 + 𝝎𝑖 × 𝑱𝑖𝝎𝑖 = 𝒇𝑖 𝜔, (28.10) for 𝑖 ∈ 𝑆. We seek a set of equations for the rigid body that combines (28.1)-(28.2) and (28.9)-(28.10) by condensing out the dependence of the slave nodes through (28.6)- (28.7). Differentiating (28.6)-(28.7) with respect to time yields 𝒙̈𝑖 = 𝒙̈ + 𝝎̇ × 𝒓𝑖 + 𝝎 × 𝝎 × 𝒓𝑖, 𝝎̇𝑖 = 𝝎̇, which can be inserted into (28.9)-(28.10) to yield 𝑚𝑖[𝒙̈ + 𝝎̇ × 𝒓𝑖] = 𝒇𝑖 𝑥 − 𝑚𝑖𝝎 × 𝝎 × 𝒓𝑖, 𝑱𝑖𝝎̇ = 𝒇𝑖 𝜔 − 𝝎 × 𝑱𝑖𝝎. This can be compactly written as [ 𝑚𝑖 −𝑚𝑖𝑹𝑖 𝑱𝑖 ] [ 𝒙̈ 𝝎̇ ] = [ 𝑥 − 𝑚𝑖𝝎 × 𝝎 × 𝒓𝑖 𝒇𝑖 𝜔 − 𝝎 × 𝑱𝑖𝝎 𝒇𝑖 ]. (28.11) (28.12) (28.13) (28.14) (28.15) It remains to use the principle of virtual work, employing (28.8), to reduce the number of equations (rigid body and slave nodes) to the generalized rigid body equations. The result of this endeavor is (𝑀𝜌 + ∑ 𝑚𝑖 𝑖∈𝑆 )𝒙̈ − (∑ 𝑚𝑖𝑹𝑖 𝑖∈𝑆 )𝝎̇ = 𝒇𝜌 𝑥 + ∑ (𝒇𝑖 𝑥 − 𝑚𝑖𝝎 × 𝝎 × 𝒓𝑖) 𝑖∈𝑆 , (28.16) −(∑ 𝑚𝑖𝑹𝑖 𝑖∈𝑆 )𝒙̈ + (𝑱𝜌 + ∑ 𝑱𝑖 𝜔 + ∑ (𝒇𝑖 + ∑ 𝑚𝑖𝑹𝑖 𝑖∈𝑆 𝑖∈𝑆 𝜔 − 𝝎 × 𝑱𝑖𝝎) = 𝒇𝜌 )𝝎̇ 𝑇𝑹𝑖 − ∑ 𝑹𝑖 𝑖∈𝑆 𝑖∈𝑆 𝑇(𝒇𝑖 𝑥 − 𝑚𝑖𝝎 × 𝝎 × 𝒓𝑖) − 𝝎 × 𝑱𝜌𝝎, (28.17) A simplified expression can be obtained through the variable substitution 𝒛 = 𝒙 + ∑ 𝑚𝑖𝒓𝑖 𝑖∈𝑆 . (28.18) This yields 𝒙̈ = 𝒛̈ + 𝑹𝑧−𝑥𝝎̇ − 𝝎 × 𝝎 × 𝒓𝑧−𝑥 where 𝒓𝑧−𝑥 = 𝒛 − 𝒙 and 𝑹𝑧−𝑥𝒓 = 𝒓𝑧−𝑥 × 𝒓 for an arbitrary vector 𝒓. This can be inserted into (28.16) and (28.17) to provide where 𝑀𝒛̈ = 𝒇 𝑥, 𝑱𝝎̇ = 𝒇 𝜔. 𝑀 = 𝑀𝜌 + ∑ 𝑚𝑖 𝑖∈𝑆 , 𝒇 𝑥 = 𝒇𝜌 𝑥 + ∑ 𝒇𝑖 𝑖∈𝑆 , 𝑱 = 𝑱𝜌 + ∑ 𝑱𝑖 𝑖∈𝑆 + ∑ 𝑚𝑖𝑹𝑖 𝑖∈𝑆 𝑇𝑹𝑖 − 𝑀𝑹𝑧−𝑥 𝑇 𝑹𝑧−𝑥, (28.19) (28.20) (28.21) (28.22) (28.23) Rigid Body Dynamics LS-DYNA Theory Manual 𝒇 𝜔 = −𝝎 × 𝑱𝝎 + 𝒇𝜌 𝜔 + ∑ (𝒇𝑖 𝜔 + 𝒓𝑖 × 𝒇𝑖 𝑥) 𝑖∈𝑆 − 𝒓𝑧−𝑥 × 𝒇 𝑥. (28.24) Equations (28.19)-(28.24) are the generalized rigid body equations to be solved for 𝒙 and 𝑸, cf. (28.5) and (28.18). The mass in (28.21) and inertia tensor in (28.23) are the physical mass and physical inertia augmented by slave node properties; nodal masses 𝑚𝑖, inertias 𝑱𝑖 and locations 𝒙𝑖. We denote 𝑀 the algorithmic mass, which may not reflect what the user intuitively expects when using *MAT_RIGID to make a part rigid. Similarly 𝑱 is the algorithmic inertia tensor, and it is worth noting that a nodal rigid body must therefore be connected to deformable elements or otherwise 𝑀 = 0 and 𝑱 = 𝟎 and its whereabouts will be impossible to determine. For no mass scaling, all these properties are constant (except for rotational updates of the inertia tensors) and can essentially be calculated at time zero. If mass scaling is active, the slave nodal masses and inertias include the added mass due to mass scaling and therefore change over time. This means that inertia properties should be recomputed every time step to account for these changes, but the default behavior is that this is done only for nodal rigid bodies and not for regular rigid bodies. Presumably this is based on the assumption that the influence from slave nodes is significant for nodal rigid bodies and not so much for regular rigid bodies, which is probably true as long as the number of contiguous nodes is small compared to the total number of nodes in the rigid body. Nevertheless, with RBSMS = 1 on *CONTROL_RIGID, these extra masses are accounted for and equations (28.19)-(28.24) are solved as expressed herein. This amounts to transforming 𝒙 to 𝒛 before the update, then update 𝒛, and transform back to obtain the new 𝒙. As we now turn to the algorithmic update of the rigid body location, we restrict ourselves to a special case for the sake of simplifying the exposition; 1.We neglect mass scaling. 2.Physical properties are not defined by *PART_INERTIA. 3.The rigid body is not connected to deformable elements. 4.No lumped masses are present. which means that 𝒛 = 𝒙. From (28.19)-(28.20) can readily solve for the rigid body accelerations 𝒇 𝑥 𝒙̈ = , It turns out that the algorithmic mass 𝑀 can be calculated as 𝝎̇ = 𝑱−1 𝒇 𝜔. 𝑀 = ∑ 𝑀𝑖 𝑖∈𝑆 , (28.25) (28.26) (28.27) LS-DYNA Theory Manual Rigid Body Dynamics where 𝑀𝑖 is the mass of node 𝑖 as obtained from the mass of its associated elements (integrating material density 𝜌 by shape functions 𝜑𝑖 over element domain). Furthermore 𝒙 can be approximated from 𝑀𝒙 = ∑ 𝑀𝑖𝒙𝑖 𝑖∈𝑆 . (28.28) Likewise, the inertia tensor is approximated by a nodal summation of the product of the point masses with their moment arms 𝑱 = ∑ 𝑀𝑖𝑹𝑖 𝑖∈𝑆 𝑇𝑹𝑖 . (28.29) The initial velocities of the slave nodes are readily calculated for a rigid body from (28.6). For arbitrary orientations of the body, the inertia tensor is transformed each time step based on the incremental rotations using the standard rules of second-order tensors: 𝑱𝑛+1 = 𝑨𝑱𝑛𝑨𝑇 (28.30) where 𝑱𝑛+1 is the updated inertia tensor components in the global frame. The transformation matrix 𝑨 is not stored since the formulation is incremental, but recomputed as explained below. After calculating the rigid body accelerations from Equation (28.25) and (28.26), the rigid body translational and rotational increment, ∆𝒙 and ∆𝜽, can be calculated using the time step ∆𝑡 and the explicit time integration update. The translational coordinate is then updated as and ∆𝜽 is used to calculate 𝑨 in (28.30) using the Hughes-Winget algorithm, 𝒙𝑛+1 = 𝒙𝑛 + ∆𝒙 𝑨 = 𝑰 + 1 + ∆𝜽𝑇∆𝜽 (𝑰 + 𝛥𝑺) 𝛥𝑺, 𝛥𝑺𝒓 = ∆𝜽 × 𝒓, ∀𝒓. The coordinates of the slave nodes are incrementally updated 𝑛+1 = 𝒙𝑖 𝒙𝑖 𝑛, 𝑛 + ∆𝒙 + (𝑨 − 𝑰)𝒓𝑖 and the velocities of the nodes are calculated by differencing the coordinates 𝒙̇𝑖 = (𝒙𝑖 𝑛+1 − 𝒙𝑖 𝛥𝑡 𝑛) . (28.31) (28.32) (28.33) (28.34) (28.35) A direct integration of the rigid body accelerations into velocity and displacements is not used for two reasons: (1) calculating the rigid body accelerations of the nodes is more expensive than the current algorithm, and (2) the second-order accuracy of the central difference integration method would introduce distortion into the rigid bodies. Since the accelerations are not needed within the program, they are calculated by a post-processor using a difference scheme similar to the above. Rigid Body Dynamics LS-DYNA Theory Manual 28.1 Rigid Body Joints 28.1.1 Penalty types The joints for the rigid bodies in LS-DYNA, see Figure 28.1, are implemented using the penalty method. Given a constraint equation 𝐶(𝑥𝑖, 𝑥𝑗) = 0, for nodes 𝑖 and 𝑗, the penalty function added to the Lagrangian of the system is −1/2𝑘𝐶2(𝑥𝑖, 𝑥𝑗). The resulting nodal forces are: 𝑓𝑖 = −𝑘𝐶(𝑥𝑖, 𝑥𝑗) 𝑓𝑗 = −𝑘𝐶(𝑥𝑖, 𝑥𝑗) ∂𝐶(𝑥𝑖, 𝑥𝑗) , ∂𝑥𝑖 ∂𝐶(𝑥𝑖, 𝑥𝑗) . ∂𝑥𝑗 (28.36) (28.37) The forces acting at the nodes have to convert into forces acting on the rigid bodies. Recall that velocities of a node i is related to the velocity of the center of mass of a rigid body by Equation (28.6). By using Equation (28.6) and virtual power arguments, it may be shown that the generalized forces are: 𝑥 = 𝑓𝑖, 𝐹𝑖 𝜔 = 𝑒𝑖𝑗𝑘𝑥̅𝑗𝑓𝑘, 𝐹𝑖 (28.38) (28.39) which are the forces and moments about the center of mass. The magnitude of the penalty stiffness 𝑘 is chosen so that it does not control the stable time step size. For the central difference method, the stable time step Δ𝑡 is restricted by the condition that, Δ𝑡 = , (28.40) where 𝛺 is the highest frequency in the system. The six vibrational frequencies associated with each rigid body are determined by solving their eigenvalue problems assuming 𝑘 = 1. For a body with 𝑚 constraint equations, the linearized equations of the translational degrees of freedom are 𝑀𝑋̈ + 𝑚𝑘𝑋 = 0, (28.41) and the frequency is √𝑚𝑘/𝑀 where 𝑀 is the mass of the rigid body. The corresponding rotational equations are 𝐉𝛉̈ + 𝐊𝛉 = 0, (28.42) 𝐉 is the inertia tensor and 𝐊 is the stiffness matrix for the moment contributions from the penalty constraints. The stiffness matrix is derived by noting that the moment contribution of a constraint may be approximated by 28-6 (Rigid Body Dynamics) 𝐅𝑥 = −k𝐫𝑖 × (𝛉 × 𝐫𝑖), LS-DYNA Theory Manual Rigid Body Dynamics and noting the identity, so that 𝐫𝑖 = 𝐱𝑖 − 𝐗cm, 𝐀 × (𝐁 × 𝐂) = |𝐀 ⋅ 𝐂 − 𝐀 ⊗ 𝐂|𝐁, 𝐾 = ∑ 𝑘[𝐫𝑖 ⋅ 𝐫𝑖 − 𝐫𝑖 ⊗ 𝐫𝑖] . 𝑖=1 (28.44) (28.45) (28.46) The rotational frequencies are the roots of the equation det∣𝐊 − 𝛺2𝐉∣ = 0, which is cubic in 𝛺2. Defining the maximum frequency over all rigid bodies for 𝑘 = 1 as 𝛺max, and introducing a time step scale factor TSSF, the equation for 𝑘 is 𝑘 ≤ ( 2TSSF Δ𝑡Ωmax ) , (28.47) The joint constraints are defined in terms of the displacements of individual nodes. Regardless of whether the node belongs to a solid element or a structural element, only its translational degrees of freedom are used in the constraint equations. A spherical joint is defined for nodes 𝑖 and 𝑗 by the three constraint equations, 𝑥1𝑖 − 𝑥1𝑗 = 0 𝑥2𝑖 − 𝑥2𝑗 = 0 𝑥3𝑖 − 𝑥3𝑗 = 0, (28.48) and a revolute joint, which requires five constraints, is defined by two spherical joints, for a total of six constraint equations. Since a penalty formulation is used, the redundancy in the joint constraint equations is unimportant. A cylindrical joint is defined by taking a revolute joint and eliminating the penalty forces along the direction defined by the two spherical joints. In a similar manner, a planar joint is defined by eliminating the penalty forces that are perpendicular to the two spherical joints. The translational joint is a cylindrical joint that permits sliding along its axis, but not rotation. An additional pair of nodes is required off the axis to supply the additional constraint. The only force active between the extra nodes acts in the direction normal to the plane defined by the three pairs of nodes. The universal joint is defined by four nodes. Let the nodes on one body be 𝑖 and 𝑘, and the other body, 𝑗 and 𝑙. Two of them, 𝑖 and 𝑗, are used to define a spherical joint for the first three constraint equations. The fourth constraint equation is, 𝐶(𝑥𝑖, 𝑥𝑗, 𝑥𝑘, 𝑥𝑙) = (𝑥𝑘 − 𝑥𝑖) ⋅ (𝑥𝑖 − 𝑥𝑗) = 0, and is differentiated to give the penalty forces 𝑓𝑛 = −𝑘𝐶 ∂𝐶 ∂𝑥𝑛 four nodes numbers. (28.49) , where 𝑛 ranges over the Rigid Body Dynamics LS-DYNA Theory Manual Figure 28.1. Rigid body joints in LS-DYNA. 28.1.2 Lagrange multiplier types An alternate version of joints is to use constraints and associated Lagrange multipliers. To this end, we recall the numerical update of the rigid body kinematics. Given translational and rotational accelerations 𝒙̈ and 𝝎̇, we have and 𝒙̇ = 𝒙̇𝑛 + ∆𝑡𝑛+1/2𝒙̈ 𝒙 = 𝒙𝑛 + ∆𝑡𝑛+1𝒙̇ 𝝎 = 𝝎𝑛 + ∆𝑡𝑛+1/2𝝎̇ 𝑸 = (𝑰 − −1 ∆𝑡𝑛+1𝑹(𝝎)) (𝑰 + ∆𝑡𝑛+1𝑹(𝝎)) 𝑸𝑛 (28.50) (28.51) (28.52) (28.53) where ∆𝑡𝑛+1/2 = (∆𝑡𝑛+1 + ∆𝑡𝑛)/2 and 𝑹(𝝎)𝒗 = 𝝎 × 𝒗 for an arbitrary vector 𝒗. Here 𝑸 = [𝒒1 𝒒2 𝒒3] is the orthonormal system attached to the rigid body, which we for simplicity assume is aligned with whatever joints we are considering. For instance, if two bodies 𝑖 and 𝑗 are connected with a joint we let 𝑸𝑖 = 𝑸𝑗 initially, and let the vectors are aligned with the axes of the joint. Also, each body has a point 𝒑 where the system is assumed to be attached and that defines the origin of the joint. Referring to the two LS-DYNA Theory Manual Rigid Body Dynamics bodies examplified, we assume that 𝒑𝑖 = 𝒑𝑗 initially. The point 𝒑 is for simplicity expressed as 𝒑 = 𝒙 + 𝒅, where 𝒅 is a vector attached to the rigid body and updates in analogy with 𝑸, i.e., using the Hughes-Winget formula (28.53). For bodies with no constraints, the accelerations are given directly by the solution of the equations of motion for each individual body, but now we seek to solve the equations of motion with respect to the combined accelerations 𝑿̈ and 𝜴̇ of all bodies with joint constraints, subject to these constraints. This can be written as 𝑴𝑿̈ − 𝑭𝑥 = 𝟎 𝑱𝛀̇ − 𝑭𝜃 = 𝟎 (28.54) (28.55) where we have collected quantities for all bodies of interest to form a complete system. Here 𝑴 is the mass matrix, 𝑱 is the inertia matrix while 𝑭𝑥 and 𝑭𝜃 are the external forces and torques coming from all other features in the model. The constraints can be written and a Lagrangian system is set up as 𝑪(𝑿̈ , 𝜴̇) = 𝟎, 𝑴𝑿̈ − 𝑭𝑥 + ( ) 𝜕𝑪 𝜕𝑿̈ 𝜦 = 𝟎 𝑱𝜴̇ − 𝑭𝜃 + ( 𝜕𝑪 𝜕𝜴̇ ) 𝜦 = 𝟎, (28.56) (28.57) (28.58) with 𝜦 being the Lagrange multiplier. In the quest for a solution, we linearize this to form a Newton step according to 𝑴Δ𝑿̈ + {⎧ 𝜕 𝜕𝑿̈ ⎩{⎨ ( ) Δ𝑿̈ + 𝜕𝑪 𝜕𝑿̈ }⎫ ⎭}⎬ = 𝑭𝑥 − 𝑴𝑿̈ − ( {⎧ 𝜕 𝜕𝛀̇ ⎩{⎨ 𝜕𝑪 𝜕𝑿̈ ) 𝜦 ) ( 𝜕𝑪 𝜕𝑿̈ }⎫ ⎭}⎬ Δ𝛀̇ + ( 𝜕𝑪 𝜕𝑿̈ ) Δ𝜦 𝑱𝛥𝜴̇ + {⎧ 𝜕 𝜕𝑿̈ ⎩{⎨ ( ) 𝜕𝑪 𝜕𝜴̇ 𝛥𝑿̈ + }⎫ ⎭}⎬ = 𝑭𝜃 − 𝑱𝜴̇ − ( {⎧ 𝜕 𝜕𝜴̇ ⎩{⎨ 𝜕𝑪 𝜕𝜴̇ ) 𝜦. ) ( 𝜕𝑪 𝜕𝜴̇ }⎫ ⎭}⎬ 𝛥𝜴̇ + ( 𝜕𝑪 𝜕𝜴̇ ) 𝛥𝜦 This is accompanied with a linearization of the constraints themselves 𝜕𝑪 𝜕𝑿̈ 𝛥𝑿̈ + 𝜕𝑪 𝜕𝜴̇ 𝛥𝜴̇ = −𝑪 (28.59) (28.60) (28.61) to form a solvable system of equations. Given a starting solution 𝑿̈ = 𝟎, 𝜴̇ = 𝟎, and 𝜦 = 𝟎, the first system to solve is simplified to Rigid Body Dynamics LS-DYNA Theory Manual 𝑴Δ𝑿̈ + ( 𝜕𝑪 𝜕𝑿̈ ) Δ𝜦 = 𝑭𝑥 𝑱𝛥𝜴̇ + ( ) 𝜕𝑪 𝜕𝜴̇ 𝛥𝜦 = 𝑭𝜃. (28.62) (28.63) This, i.e., equations (28.61)-(28.63), is a standard symmetric Lagrange system of equations, and is often sufficient to yield an accurate solution without iterating. However, due to nonlinearity 𝑪 may grow and therefore a fully iterative scheme is performed according at a time step frequency given by an internal rule. For simplicity, the approximation 𝜦 ≈ 𝟎 is maintained for the setup of the system matrix to avoid the second derivative of constraints and a more complex nonsymmetric system. For the right hand side we make no such approximation. Some of the joint constraints of interest are Spherical joint Revolute joint Cylindrical joint Planar joint 𝒑𝑖 − 𝒑𝑗 = 𝟎 𝒑𝑖 − 𝒑𝑗 = 𝟎 𝑖 ∙ 𝒒2 𝒒1 𝑗 = 𝒒3 𝑖 ∙ 𝒒1 𝑗 = 0 𝑖 ∙ (𝒑𝑖 − 𝒑𝑗) = 𝒒3 𝒒2 𝑖 ∙ (𝒑𝑖 − 𝒑𝑗) = 0 𝑖 ∙ 𝒒2 𝒒1 𝑗 = 𝒒3 𝑖 ∙ 𝒒1 𝑗 = 0 𝑖 ∙ (𝒑𝑖 − 𝒑𝑗) = 0 𝒒1 𝑖 ∙ 𝒒2 𝒒1 𝑗 = 𝒒3 𝑖 ∙ 𝒒1 𝑗 = 0 Translational joint 𝑖 ∙ (𝒑𝑖 − 𝒑𝑗) = 𝒒3 𝒒2 𝑖 ∙ (𝒑𝑖 − 𝒑𝑗) = 0 𝑖 ∙ 𝒒2 𝒒1 𝑗 = 𝒒2 𝑖 ∙ 𝒒3 𝑗 = 𝒒3 𝑖 ∙ 𝒒1 𝑗 = 0 (28.64) (28.65) (28.66) (28.67) (28.68) (28.69) (28.70) (28.71) (28.72) To form the system of equations, the first order sensitivities needed are those of 𝑸, 𝒙 and 𝒅, and can be expressed as LS-DYNA Theory Manual Rigid Body Dynamics 𝛿𝒒𝑖 = ∆𝑡𝑛+1 (𝑰 − −1 ∆𝑡𝑛+1𝑹(𝝎)) 𝛿𝝎 × ≈ ∆𝑡𝑛+1∆𝑡𝑛+1/2𝛿𝝎̇ × 𝒒𝑖 {⎧ ⎩{⎨ (𝑰 − −1 ∆𝑡𝑛+1𝑹(𝝎)) 𝒒𝑖 }⎫ ⎭}⎬ 𝛿𝒅 = ⋯ ≈ ∆𝑡𝑛+1∆𝑡𝑛+1/2𝛿𝝎̇ × 𝒅 𝛿𝒙 = ∆𝑡𝑛+1∆𝑡𝑛+1/2𝛿𝒙̈ (28.73) (28.74) (28.75) where we have differentiated (28.50)-(28.53) using the accelerations as independent variables. 28.2 Deformable to Rigid Material Switching Occasionally in practice, long duration, large rigid body motions arise that are prohibitively expensive to simulate if the elements in the model are deformable. Such a case could occur possibly in automotive rollover where the time duration of the rollover would dominate the cost relative to the post impact response that occurs much later. To permit such simulations to be efficiently handled a capability to switch a subset of materials from deformable to rigid and back to deformable is available. In practice the suspension system and tires would remain deformable A flag is set in the input to let LS-DYNA know that all materials in the model have the potential to become rigid bodies sometime during the calculation. When this flag is set a cost penalty is incurred on vector machines since the blocking of materials in the element loops will be based on the part ID rather than the material type ID. Normally this cost is insignificant relative to the cost reduction due to this unique feature. For rigid body switching to work properly the choice of the shell element formulation is critical. The Hughes-Liu elements cannot currently be used for two reasons. First, since these elements compute the strains from the rotations of the nodal fiber vectors from one cycle to the next, the nodal fiber vectors should be updated with the rigid body motions and this is not done. Secondly, the stresses are stored in the global system as opposed to the co-rotational system. Therefore, the stresses would also need to be transformed with the rigid body motions or zeroed out. The co-rotational elements of Belytschko and co-workers do not reference nodal fibers for the strain computations and the stresses are stored in the co-rotational coordinate system which eliminates the need for the transformations; consequently, these elements can be safely used. The membrane elements and airbag elements are closely related to the Belytschko shells and can be safely used with the switching options. The beam elements have nodal triads that are used to track the nodal rotations and to calculate the deformation displacements from one cycle to the next. These nodal triads are updated every cycle with the rigid body rotations to prevent non-physical Rigid Body Dynamics LS-DYNA Theory Manual behavior when the rigid body is switched back to deformable. This applies to all beam element formulations in LS-DYNA. The Belytschko beam formulations are preferred for the switching options for like the shell elements, the Hughes-Liu beams keep the stresses in the global system. Truss elements like the membrane elements are trivially treated and pose no difficulties. The brick elements store the stresses in the global system and upon switching the rigid material to deformable the element stresses are zeroed to eliminate spurious behavior. The implementation addresses many potential problems and has worked well in practice. The current restrictions can be eliminated if the need arises and anyway should pose no insurmountable problems. We will continue to improve this capability if we find that it is becoming a popular option. 28.3 Rigid Body Welds The weld capability in LS-DYNA is based on rigid body dynamics. Each weld is defined by a set of nodal points which moves rigidly with six degrees of freedom until a failure criteria is satisfied. Five weld options are implemented including: •Spot weld. •Fillet weld •Butt weld •Cross fillet weld •General weld Welds can fail three ways: by ductile failure which is based on the effective plastic strain, by brittle failure which is based on the force resultants acting on the rigid body weld, and by a failure time which is specified in the input. When effective plastic strain is used the weld fails when the nodal plastic strain exceeds the input value. A least squares algorithm is used to generate the nodal values of plastic strains at the nodes from the element integration point values. The plastic strain is integrated through the element and the average value is projected to the nodes with a least square fit. In the resultant based brittle failure the resultant forces and moments on each node of the weld are computed. These resultants are checked against a failure criterion which is expressed in terms of these resultants. The forces may be averaged over a user specified number of time steps to eliminate breakage due to spurious noise. After all nodes of a weld are released the rigid body is removed from the calculation. LS-DYNA Theory Manual Rigid Body Dynamics node 2 node 1 node 3 node 2 2 node spotweld 3 node spotweld node 1 node n node n-1 n node spotweld node 2 node 1 Figure 28.2. Nodal ordering and orientation of the local coordinate system is important for determining spotweld failure. Spotwelds are shown in Figure 28.2. Spotweld failure due to plastic straining p . This option occurs when the effective nodal plastic strain exceeds the input value, 𝜀fail can model the tearing out of a spotweld from the sheet metal since the plasticity is in the material that surrounds the spotweld, not the spotweld itself. This option should only be used for the material models related to metallic plasticity and can result is slightly increased run times. Brittle failure of the spotwelds occurs when: ( max(𝑓𝑛, 0) 𝑆𝑛 ) + ( ∣𝑓𝑠∣ 𝑆𝑠 ) ≥ 1, (28.76) where 𝑓𝑛 and 𝑓𝑠 are the normal and shear interface force. Component 𝑓𝑛 contributes for tensile values only. When the failure time, 𝑡f, is reached the nodal rigid body becomes Rigid Body Dynamics LS-DYNA Theory Manual inactive and the constrained nodes may move freely. In Figure 28.2 the ordering of the nodes is shown for the 2 and 3 noded spotwelds. This order is with respect to the local coordinate system where the local 𝑧 axis determines the tensile direction. The nodes in the spotweld may coincide but if they are offset the local system is not needed since the 𝑧-axis is automatically oriented based on the locations of node 1, the origin, and node 2. The failure of the 3 noded spotweld may occur gradually with first one node failing and later the second node may fail. For 𝑛 noded spotwelds the failure is progressive starting with the outer nodes (1 and 𝑛) and then moving inward to nodes 2 and 𝑛 − 1. Progressive failure is necessary to preclude failures that would create new rigid bodies. Ductile fillet weld failure, due to plastic straining, is treated identically to spotweld failure. Brittle failure of the fillet welds occurs when: 𝛽√𝜎𝑛 2 + 3(𝜏𝑛 2 + 𝜏𝑡 2) ≥ 𝜎𝑓 , (28.77) where 𝜎𝑛 = normal stress 𝜏𝑛 = shear stress in direction of weld (local 𝑦) 𝜏𝑡 = shear stress normal to weld (local 𝑥) 𝜎𝑓 = failure stress 𝛽 = failure parameter Component 𝜎𝑛 is nonzero for tensile values only. When the failure time, 𝑡𝑓 , is reached the nodal rigid body becomes inactive and the constrained nodes may move local coordinate system 2 node fillet weld 3 node fillet weld Figure 28.3. Nodal ordering and orientation of the local coordinate system is shown for fillet weld failure. 28-14 (Rigid Body Dynamics) LS-DYNA Theory Manual Rigid Body Dynamics z1 y1 x1 y2 z2 x2 z3 x3 y3 Figure 28.5. A simple cross fillet weld illustrates the required input. Here NFW = 3 with nodal pairs (A = 2, B = 1), (A = 3, B = 1), and (A = 3, B = 2). The local coordinate axes are shown. These axes are fixed in the rigid body and are referenced to the local rigid body coordinate system which tracks the rigid body rotation. freely. In Figure 28.3 the ordering of the nodes is shown for the 2 node and 3 node fillet welds. This order is with respect to the local coordinate system where the local z axis determines the tensile direction. The nodes in the fillet weld may coincide. The failure of the 3 node fillet weld may occur gradually with first one node failing and later the second node may fail. In Figure 28.4 the butt weld is shown. Ductile butt weld failure, due to plastic straining, is treated identically to spotweld failure. Brittle failure of the butt welds occurs when: 𝛽√𝜎𝑛 2 + 3(𝜏𝑛 2 + 𝜏𝑡 2) ≥ 𝜎𝑓 , (28.78) where 𝜎𝑛 = normal stress 𝜏𝑛 = shear stress in direction of weld (local y) 𝜏𝑡 = shear stress normal to weld (local z) 𝜎𝑓 = failure stress 𝛽 = failure parameter Component 𝜎𝑛 is nonzero for tensile values only. When the failure time, 𝑡𝑓 , is reached the nodal rigid body becomes inactive and the constrained nodes may move freely. The nodes in the butt weld may coincide. Rigid Body Dynamics LS-DYNA Theory Manual The cross fillet weld and general weld are shown in Figures 28.5 and 28.6, respectively. The treatment of failure for these welds is based on the formulation for the fillet and butt welds. Figure 28.6. A general weld is a mixture of fillet and butt welds. LS-DYNA Theory Manual Contact-Impact Algorithm 29 Contact-Impact Algorithm 29.1 Introduction The treatment of sliding and impact along interfaces has always been an important capability in DYNA3D and more recently in LS-DYNA. Three distinct methods for handling this have been implemented, which we will refer to as the kinematic constraint method, the penalty method, and the distributed parameter method. Of these, the first approach is now used for tying interfaces. The relative merits of each approach are discussed below. Interfaces can be defined in three dimensions by listing in arbitrary order all triangular and quadrilateral segments that comprise each side of the interface. One side of the interface is designated as the slave side, and the other is designated as the master side. Nodes lying in those surfaces are referred to as slave and master nodes, respectively. In the symmetric penalty method, this distinction is irrelevant, but in the other methods the slave nodes are constrained to slide on the master surface after impact and must remain on the master surface until a tensile force develops between the node and the surface. Today, automatic contact definitions are commonly used. In this approach the slave and master surfaces are generated internally within LS-DYNA from the part ID's given for each surface. For automotive crash models it is quite common to include the entire vehicle in one single surface contact definition where the all the nodes and elements within the interface can interact. 29.2 Kinematic Constraint Method The kinematic constraint method which uses the impact and release conditions of Hughes et al., [1976] was implemented first in DYNA2D [Hallquist 1976b] and finally Contact-Impact Algorithm LS-DYNA Theory Manual extended to three dimensions in DYNA3D. Constraints are imposed on the global equations by a transformation of the nodal displacement components of the slave nodes along the contact interface. This transformation has the effect of eliminating the normal degree of freedom of nodes. To preserve the efficiency of the explicit time integration, the mass is lumped to the extent that only the global degrees of freedom of each master node are coupled. Impact and release conditions are imposed to insure momentum conservation. The release conditions are of academic interest and were quickly removed from the coding. Problems arise with this method when the master surface zoning is finer than the slave surface zoning as shown in two dimensions in Figure 29.1. Here, certain master nodes can penetrate through the slave surface without resistance and create a kink in the slide line. Such kinks are relatively common with this formulation, and, when interface pressures are high, these kinks occur whether one or more quadrature points are used in the element integration. It may be argued, of course, that better zoning would minimize such problems; but for many problems that are of interest, good zoning in the initial configuration may be very poor zoning later. Such is the case, for example, when gaseous products of a high explosive gas expand against the surface of a structural member. 29.3 Penalty Method The penalty method is used in the explicit programs DYNA2D and DYNA3D as well as in the implicit programs NIKE2D and NIKE3D. The method consists of placing normal interface springs between all penetrating nodes and the contact surface. With the exception of the spring stiffness matrix which must be assembled into the global stiffness matrix, the implicit and explicit treatments are similar. The NIKE2D/3D and DYNA2D/3D programs compute a unique modulus for the element in which it resides. In our opinion, pre-empting user control over this critical parameter greatly increases slave surface master surface Indicates nodes treated as free surface nodes Figure 29.1. Nodes of the master slide surface designated with an “x” are treated as free surface nodes in the nodal constraint method. the success of the method. LS-DYNA Theory Manual Contact-Impact Algorithm Quite in contrast to the nodal constraint method, the penalty method approach is found to excite little if any mesh hourglassing. This lack of noise is undoubtedly attributable to the symmetry of the approach. Momentum is exactly conserved without the necessity of imposing impact and release conditions. Furthermore, no special treatment of intersecting interfaces is required, greatly simplifying the implementation. Currently three implementations of the penalty algorithm are available: • Standard Penalty Formulation • Soft Constraint Penalty Formulation, which has been implemented to treat contact between bodies with dissimilar material properties (e.g. steel-foam). Stiffness calculation and its update during the simulation differs from the Stand- ard Penalty Formulation. • Segment-based Penalty Formulation, it is a powerful contact algorithm whose logic is a slave segment-master segment approach instead of a traditional slave node-master segment approach. This contact has proven very useful for airbag self-contact during inflation and complex contact conditions. In the standard penalty formulation, the interface stiffness is chosen to be approximately the same order of magnitude as the stiffness of the interface element normal to the interface. Consequently the computed time step size is unaffected by the existence of the interfaces. However, if interface pressures become large, unacceptable penetration may occur. By scaling up the stiffness and scaling down the time step size, we may still solve such problems using the penalty approach. Since this increases the number of time steps and hence the cost, a sliding-only option has been implemented for treating explosive-structure interaction problems thereby avoiding use of the penalty approach. This latter option is based on a specialization of the third method described below. 29.4 Distributed Parameter Method This method is used in DYNA2D, and a specialization of it is the sliding only option in DYNA3D. Motivation for this approach came from the TENSOR [Burton et. al., 1982] and HEMP [Wilkins 1964] programs which displayed fewer mesh instabilities than DYNA2D with the nodal constraint algorithm. The first DYNA2D implementation of this last algorithm is described in detail by Hallquist [1978]. Since this early publication, the method has been moderately improved but the major ideas remain the same. Contact-Impact Algorithm LS-DYNA Theory Manual b1 ∂b1 ∂b2 b2 ∂B1 B1 ∂B2 B2 Figure 29.2. Reference and deformed configuration. In the distributed parameter formulation, one-half the slave element mass of each element in contact is distributed to the covered master surface area. Also, the internal stress in each element determines a pressure distribution for the master surface area that receives the mass. After completing this distribution of mass and pressure, we can update the acceleration of the master surface. Constraints are then imposed on slave node accelerations and velocities to insure their movement along the master surface. Unlike the finite difference hydro programs, we do not allow slave nodes to penetrate; therefore we avoid “put back on” logic. In another simplification, our calculation of the slave element relative volume ignores any intrusion of the master surfaces. The HEMP and TENSOR codes consider the master surface in this calculation. 29.5 Preliminaries Consider the time-dependent motion of two bodies occupying regions B1 and B2 in their undeformed configuration at time zero. Assume that the intersection B1 ∩ B2 = 0, (29.1) is satisfied. Let 𝜕B1 and ∂B2denote the boundaries of B1 and B2, respectively. At some later time, these bodies occupy regions b1 and b2 bounded by ∂b1and ∂b2as shown in Figure 29.2. Because the deformed configurations cannot penetrate, (b1 − ∂b1) ∩ b2 = 0. (29.2) LS-DYNA Theory Manual Contact-Impact Algorithm S1 ns S2 S4 ms S3 X3 X2 X1 Figure 29.3. In this figure, four master segments can harbor slave node 𝑛𝑠 given that 𝑚𝑠 is the nearest master node. As long as (∂b1 ∩ ∂b2) = 0, the equations of motion remain uncoupled. In the foregoing and following equations, the right superscript 𝛼 (= 1,2) denotes the body to which the quantity refers. Before a detailed description of the theory is given, some additional statements should be made concerning the terminology. The surfaces ∂b1 and ∂b2 of the discretized bodies b1 and b2 become the master and slave surfaces respectively. Choice of the master and slave surfaces is arbitrary when the symmetric penalty treatment is employed. Otherwise, the more coarsely meshed surface should be chosen as the master surface unless there is a large difference in mass densities in which case the side corresponding to the material with the highest density is recommended. Nodal points that define ∂b1 are called master nodes and nodes that define ∂b2 are called slave nodes. When (∂b1 ∩ ∂b2) ≠ 0, the constraints are imposed to prevent penetration. Right superscripts are implied whenever a variable refers to either the master surface ∂b1, or slave surface, ∂b2; consequently, these superscripts are dropped in the development which follows. 29.6 Slave Search The slave search is common to all interface algorithms implemented in DYNA3D. This search finds for each slave node its nearest point on the master surface. Lines drawn from a slave node to its nearest point will be perpendicular to the master surface, unless the point lies along the intersection of two master segments, where a segment is defined to be a 3- or 4-node element of a surface. Contact-Impact Algorithm LS-DYNA Theory Manual Consider a slave node, 𝑛𝑠, sliding on a piecewise smooth master surface and assume that a search of the master surface has located the master node, 𝑚𝑠, lying nearest to 𝑛𝑠. Figure 29.3 depicts a portion of a master surface with nodes 𝑚𝑠 and 𝑛𝑠 labeled. If 𝑚𝑠 and 𝑛𝑠 do not coincide, 𝑛𝑠 can usually be shown to lie in a segment 𝑠1 via the following tests: (𝐜𝑖 × 𝐬) ⋅ (𝐜𝑖 × 𝐜𝑖+1) > 0, (𝐜𝑖 × 𝐬) ⋅ (𝐬 × 𝐜𝑖+1) > 0, (29.3) where vector 𝐜𝑖 and 𝐜𝑖+1 are along edges of 𝑠1 and point outward from 𝑚𝑠. Vector 𝐬 is the projection of the vector beginning at 𝑚𝑠, ending at 𝑛𝑠, and denoted by 𝐠, onto the plane being examined . where for segment 𝑠1 𝐬 = 𝐠 − (𝐠 ⋅ 𝐦)𝐦, 𝐦 = 𝐜𝑖 × 𝐜𝑖+1 ∣𝐜𝑖 × 𝐜𝑖+1∣ . (29.4) (29.5) Since the sliding constraints keep 𝑛𝑠 close but not necessarily on the master surface and since 𝑛𝑠 may lie near or even on the intersection of two master segments, the inequalities of Equation (29.3) may be inconclusive, i.e., they may fail to be satisfied or more than one may give positive results. When this occurs 𝑛𝑠 is assumed to lie along the intersection which yields the maximum value for the quantity 𝐠 ⋅ 𝐜𝑖 |𝐜𝑖| 𝑖 = 1,2,3,4, .. (29.6) When the contact surface is made up of badly shaped elements, the segment apparently identified as containing the slave node actually may not, as shown in Figure 29.5. ns ci+1 ms X3 X2 X1 Figure 29.4. Projection of g onto master segment 𝑠1 LS-DYNA Theory Manual Contact-Impact Algorithm Figure 29.5. When the nearest node fails to contain the segment that harbors the slave node, segments numbered 1-8 are searched in the order shown. Assume that a master segment has been located for slave node 𝑛𝑠 and that 𝑛𝑠 is not identified as lying on the intersection of two master segments. Then the identification of the contact point, defined as the point on the master segment which is nearest to 𝑛𝑠, becomes nontrivial. For each master surface segment, 𝑠1 is given the parametric representation of Equation (1.7), repeated here for clarity: where 𝐫 = 𝑓1(𝜉 , 𝜂)𝐢1 + 𝑓2(𝜉 , 𝜂)𝐢2 + 𝑓3(𝜉 , 𝜂)𝐢3, 𝑓𝑖(𝜉 , 𝜂) = ∑ 𝜙𝑗𝑥𝑖 . 𝑗=1 Note that r1 is at least once continuously differentiable and that ∂𝐫 ∂𝜉 × ∂𝐫 ∂𝜂 ≠ 0, (29.7) (29.8) (29.9) Thus 𝐫 represents a master segment that has a unique normal whose direction depends continuously on the points of s1. Let t be a position vector drawn to slave node ns and assume that the master surface segment s1 has been identified with ns. The contact point coordinates (𝜉c, 𝜂c) on s1 must satisfy ∂𝐫 ∂𝜉 ∂𝐫 ∂𝜂 (𝜉𝑐, 𝜂𝑐) ⋅ [𝐭 − 𝐫(𝜉𝑐, 𝜂𝑐)] = 0, (𝜉𝑐, 𝜂𝑐) ⋅ [𝐭 − 𝐫(𝜉𝑐, 𝜂𝑐)] = 0. (29.10) (29.11) Contact-Impact Algorithm LS-DYNA Theory Manual ns X3 X2 X1 Figure 29.6. Location of contact point when ns lies above master segment. The physical problem is illustrated in Figure 29.6, which shows ns lying above the master surface. Equations (29.10) and (29.11) are readily solved for 𝜉c and 𝜂c. One way to accomplish this is to solve Equation (29.10) for 𝜉c in terms of 𝜂c, and substitute the results into Equation (29.11). This yields a cubic equation in 𝜂c which is presently solved numerically in LS-DYNA. In the near future, we hope to implement a closed form solution for the contact point. The equations are solved numerically. When two nodes of a bilinear quadrilateral are collapsed into a single node for a triangle, the Jacobian of the minimization problem is singular at the collapsed node. Fortunately, there is an analytical solution for triangular segments since three points define a plane. Newton- Raphson iteration is a natural choice for solving these simple nonlinear equations. The method diverges with distorted elements unless the initial guess is accurate. An exact contact point calculation is critical in post-buckling calculations to prevent the solution from wandering away from the desired buckling mode. Three iterations with a least-squares projection are used to generate an initial guess: [ 𝜉0 = 0, 𝜂0 = 0, 𝐫,𝜉 𝐫,𝜂 𝜉𝑖+1 = 𝜉𝑖 + Δ𝜉 , ] [𝐫,𝜉 𝐫,𝜂] { Δ𝜉 Δ𝜂 } = [ 𝐫,𝜉 𝐫,𝜂 ] {𝐫(𝜉𝑖,𝜂𝑖) − 𝐭}, (29.12) 𝜂𝑖+1 = 𝜂𝑖 + Δ𝜂, followed by the Newton-Raphson iterations which are limited to ten iterations, but which usually converges in four or less. LS-DYNA Theory Manual Contact-Impact Algorithm [H] { Δ𝜉 Δ𝜂 } = − { 𝐫,𝜉 𝐫,𝜂 [H] = { 𝐫,ξ 𝐫,η } [𝐫,𝜉 𝐫,𝜂] + [ } {𝐫(𝜉𝑖,𝜂𝑖) − 𝐭}, 𝐫 ⋅ 𝐫,𝜉𝜂 𝐫 ⋅ 𝐫,𝜉𝜂 ] , (29.13) 𝜉𝑖+1 = 𝜉𝑖 + Δ𝜉 , 𝜂𝑖+1 = 𝜂𝑖 + Δ𝜂, In concave regions, a slave node may have isoparametric coordinates that lie outside of the [−1, +1] range for all of the master segments, yet still have penetrated the surface. A simple strategy is used for handling this case, but it can fail. The contact segment for each node is saved every time step. If the slave node contact point defined in terms of the isoparametric coordinates of the segment, is just outside of the segment, and the node penetrated the isoparametric surface, and no other segment associated with the nearest neighbor satisfies the inequality test, then the contact point is assumed to occur on the edge of the segment. In effect, the definition of the master segments is extended so that they overlap by a small amount. In the hydrocode literature, this approach is similar to the slide line extensions used in two dimensions. This simple procedure works well for most cases, but it can fail in situations involving sharp concave corners. 29.7 Sliding With Closure and Separation 29.7.1 Standard Penalty Formulation Because this is perhaps the most general and most used interface algorithm, we choose to discuss it first. In applying this penalty method, each slave node is checked for penetration through the master surface. If the slave node does not penetrate, nothing is done. If it does penetrate, an interface force is applied between the slave node and its contact point. The magnitude of this force is proportional to the amount of penetration. This may be thought of as the addition of an interface spring. Penetration of the slave node ns through the master segment which contains its contact point is indicated if where 𝑙 = 𝐧𝑖 × [𝐭 − 𝐫(𝜉𝑐, 𝜂𝑐)] < 0, 𝐧𝑖 = 𝐧𝑖(𝜉𝑐, 𝜂𝑐) is normal to the master segment at the contact point. (29.14) (29.15) If slave node ns has penetrated through master segment 𝑠𝑖, we add an interface force vector 𝐟s: 𝐟𝑠 = −𝑙𝑘𝑖𝐧𝑖 if 𝑙 < 0 (29.16) Contact-Impact Algorithm LS-DYNA Theory Manual to the degrees of freedom corresponding to ns and 𝑖 = 𝜙𝑖(𝜉𝑐, 𝜂𝑐)𝑓𝑠 𝑓𝑚 if 𝑙 < 0 (29.17) to the four nodes (𝑖 = 1,2,3,4) that comprise master segment 𝑠𝑖. The stiffness factor 𝑘𝑖 for master segment 𝑠𝑖 is given in terms of the bulk modulus 𝐾𝑖, the volume 𝑉𝑖, and the face area 𝐴𝑖 of the element that contains 𝑠𝑖 as for brick elements and 𝑘𝑖 = 𝑓𝑠𝑖𝐾𝑖𝐴𝑖 𝑉𝑖 𝑘𝑖 = 𝑓𝑠𝑖𝐾𝑖𝐴𝑖 max(shell diagonal) (29.18) (29.19) for shell elements where 𝑓𝑠𝑖 is a scale factor for the interface stiffness and is normally defaulted to .10. Larger values may cause instabilities unless the time step size is scaled back in the time step calculation. In LS-DYNA, a number of options are available for setting the penalty stiffness value. This is often an issue since the materials in contact may have drastically different bulk modulii. The calculational choices are: • Minimum of the master segment and slave node stiffness. (default) • Use master segment stiffness • Use slave node value • Use slave node value, area or mass weighted. • As above but inversely proportional to the shell thickness. The default may sometimes fail due to an excessively small stiffness. When this occurs it is necessary to manually scale the interface stiffness. Care must be taken not to induce an instability when such scaling is performed. If the soft material also has a low density, it may be necessary to reduce the scale factor on the computed stable time step. 29.7.2 Soft Constraint Penalty Formulation Very soft materials have an undesired effect on the contact stiffness, lowering its value and ultimately causing excessive penetration. An alternative to put a scale factor on the contact stiffness for SOFT = 0 is to use a Soft Constraint Penalty Formulation. The idea behind this option is to eliminate the excessive penetration by using a different formulation for the contact stiffness. In addition to the master and slave contact stiffness, an additional stiffness is calculated, which is based on the stability (Courant’s criterion) of the local system LS-DYNA Theory Manual Contact-Impact Algorithm comprised of two masses (segments) connected by a spring. This is the stability contact stiffness 𝑘cs and is calculated by: 𝑘cs(𝑡) = 0.5 ⋅ SOFSCL ⋅ 𝑚∗ ⋅ ( , Δ𝑡𝑐(𝑡) ) (29.20) where SOFSCL on Optional Card A of *CONTROL_CONTACT is the scale factor for the Soft Constraint Penalty Formulation, 𝑚∗ is a function of the mass of the slave node and of the master nodes. Δ𝑡c is set to the initial solution timestep. If the solution time step grows, Δ𝑡c is reset to the current time step to prevent unstable behavior. A comparative check against the contact stiffness calculated with the traditional penalty formulation, 𝑘soft=0, and in general the maximum stiffness between the two is taken, 𝑘soft=1 = max{𝑘cs, 𝑘soft=0}. (29.21) 29.7.3 Segment-based Penalty Formulation Segment based contact is a general purpose shell and solid element penalty type contact algorithm. Segment based contact uses a contact stiffness similar to the SOFT = 1 stiffness option, but the details are quite different. 𝑘cs(𝑡) = 0.5 ⋅ SLSFAC ⋅ {⎧SFS }⎫ or SFM⎭}⎬ ⎩{⎨ ( 𝑚1𝑚2 𝑚1 + 𝑚2 ) ( ) . Δ𝑡𝑐(𝑡) (29.22) Segment masses are used rather than nodal masses. Segment mass is equal to the element mass for shell segments and half the element mass for solid element segments. Like the Soft Constraint Penalty Formulation, 𝑑𝑡 is set to the initial solution time step which is updated if the solution time step grows larger to prevent unstable behavior. However, it differs from SOFT = 1 in how 𝑑𝑡 is updated. 𝑑𝑡 is updated only if the solution time step grows by more than 5%. This allows 𝑑𝑡 to remain constant in most cases, even if the solution time step slightly grows. 29.8 Recent Improvements in Surface-to-Surface Contact A number of recent changes have been made in the surface-to-surface contact including contact searching, accounting for thickness, and contact damping. These changes have been implemented primarily to aid in the analysis of sheet metal forming problems. Contact-Impact Algorithm LS-DYNA Theory Manual closet nodal point slave node Figure 29.7. Failure to find the contact segment can be caused by poor aspect ratios in the finite element mesh. 29.8.1 Improvements to the Contact Searching In metal forming applications, problems with the contact searching were found when the rigid body stamping dies were meshed with elements having very poor aspect ratios. The nearest node algorithm described above can break down since the nearest node is not necessarily anywhere near the segment that harbors the slave node as is assumed in Figure 29.5 . Such distorted elements are commonly used in rigid bodies in order to define the geometry accurately. To circumvent the problem caused by bad aspect ratios, an expanded searching procedure is used in which we attempt to locate the nearest segment rather than the nearest nodal point. We first sort the segments based on their centroids as shown in Figure 29.8 using a one-dimensional bucket sorting technique. centroids of master contact segments search 3 bins for this slave node Figure 29.8. One-dimensional bucket sorting identifies the nearest segments for each slave node. LS-DYNA Theory Manual Contact-Impact Algorithm Figure 29.9. Interior points are constructed in the segments for determining the closest point to the slave node. Once a list of possible candidates is identified for a slave node, it is necessary to locate the possible segments that contain the slave node of interest. For each quadrilateral segment, four points are constructed at the centroids of the four triangles each defined by 3 nodes as shown in Figure 29.9 where the black point is the centroid of the quadrilateral. These centroids are used to find the nearest point to the slave node and hence the nearest segment. The nodes of the three nearest segments are then examined to identify the three nearest nodes. Just one node from each segment is allowed to be a nearest node. When the nearest segment fails to harbor the slave node, the adjacent segments are checked. The old algorithm checks the segments labeled 1-3 (Figure 29.10), which do not contain the slave node, and fails. closet nodal point slave node segment identified as containing slave node Figure 29.10. In case the stored segment fails to contain the node, the adjacent segments are checked. Contact-Impact Algorithm LS-DYNA Theory Manual Projected contact surface length of projection vector is 1/2 the shell thickness Figure 29.11. Contact surface is based on mid-surface normal projection vectors. 29.8.2 Accounting For the Shell Thickness Shell thickness effects are important when shell elements are used to model sheet metal. Unless thickness is considered in the contact, the effect of thinning on frictional interface stresses due to membrane stretching will be difficult to treat. In the treatment of thickness we project both the slave and master surfaces based on the mid-surface normal projection vectors as shown in Figure 29.11. The surfaces, therefore, must be offset by an amount equal to 1/2 their total thickness (Figure 29.12). This allows DYNA3D to check the node numbering of the segments automatically to ensure that the shells are properly oriented. Thickness changes in the contact are accounted for if and only if the shell thickness change option is flagged in the input. Each cycle, as the shell elements are processed, the nodal thicknesses are stored for use in the contact algorithms. The interface stiffness may change with thickness depending on the input options used. Figure 29.12. The slave and master surfaces must be offset in the input by one-half the total shell thickness. This also allows the segments to be oriented automatically. LS-DYNA Theory Manual Contact-Impact Algorithm Type 5 contact considers nodes interacting with a surface. This algorithm calls exactly the same subroutines as surface-to-surface but not symmetrically: i.e., the subroutines are called once, not twice. To account for the nodal thickness, the maximum shell thickness of any shell connected to the node is taken as the nodal thickness and is updated every cycle. The projection of the node is done normal to the contact surface as shown in Figure 29.13. 29.8.3 Initial Contact Interpenetrations The need to offset contact surfaces to account for the thickness of the shell elements contributes to initial contact interpenetrations. These interpenetrations can lead to severe numerical problems when execution begins so they should be corrected if LS-DYNA is to run successfully. Often an early growth of negative contact energy is one sign that initial interpenetrations exist. Currently, warning messages are printed to the terminal, the D3HSP file, and the MESSAG file to report interpenetrations of nodes through contact segments and the modifications to the geometry made by LS-DYNA to eliminate the interpenetrations. Sometimes such corrections simply move the problem elsewhere since it is very possible that the physical location of the shell mid-surface and possibly the shell thickness are incorrect. In the single surface contact algorithms any nodes still interpenetrating on the second time step are removed from the contact with a warning message. In some geometry's interpenetrations cannot be detected since the contact node interpenetrates completely through the surface at the beginning of the calculation. This is illustrated in Figure 29.14. Another case contributing to initial interpenetrations occurs when the edge of a shell element is on the surface of a solid material as seen in Figure 29.15. Currently, shell edges are rounded with a radius equal to one-half the 1/2 thickness of node Projected contact surface length of projection vector is 1/2 the shell thickness Figure 29.13. In a type 5 contact, thickness can also be taken into account. shell thickness. Contact-Impact Algorithm LS-DYNA Theory Manual Detected Penetration Undetected Penetration Figure 29.14. Undetected interpenetration. Such interpenetrations are frequently due to the use of coarse meshes. To avoid problems with initial interpenetrations, the following recommendations should be considered: •Adequately offset adjacent surfaces to account for part thickness during the mesh generation phase. •Use consistently refined meshes on adjacent parts which have significant curva- tures. •Be very careful when defining thickness on shell and beam section definitions -- especially for rigid bodies. •Scale back part thickness if necessary. Scaling a 1.5mm thickness to .75mm should not cause problems but scaling to .075mm might. Alternatively, de- fine a smaller contact thickness by part ID. Warning: if the part is too thin contact failure will probably occur •Use spot welds instead of merged nodes to allow the shell mid surfaces to be offset. 29.8.4 Contact Energy Calculation Contact energy, 𝐸contact, is incrementally updated from time 𝑛 to time 𝑛 + 1 for each contact interface as: Brick shell Inner penetration if edge is too close Figure 29.15. Undetected interpenetration due to rounding the edge of the shell element. LS-DYNA Theory Manual Contact-Impact Algorithm Figure 29.16. Hemispherical deep drawing problem. 𝑛+1 = 𝐸contact 𝐸contact 𝑛𝑠𝑛 + [∑ Δ𝐹𝑖 𝑖=1 slave × Δ𝑑𝑖𝑠𝑡𝑖 𝑛𝑚𝑛 slave + ∑ Δ𝐹𝑖 𝑖=1 master 𝑛+1 × Δ𝑑𝑖𝑠𝑡𝑖 master] , (29.23) slave is where 𝑛𝑠𝑛 is the number of slave nodes, 𝑛𝑚𝑛 is the number of master nodes, Δ𝐹𝑖 master is the the interface force between the ith slave node and the contact segment Δ𝐹𝑖 slave is the interface force between the ith master node and the contact segment, Δ𝑑𝑖𝑠𝑡𝑖 incremental distance the ith slave node has moved during the current time step, and master is the incremental distance the ith master node has moved during the current Δ𝑑𝑖𝑠𝑡𝑖 time step. In the absence of friction the slave and master side energies should be close in magnitude but opposite in sign. The sum, 𝐸contact, should equal the stored energy. Large negative contact energy is usually caused by undetected penetrations. Contact energies are reported in the SLEOUT file. In the presence of friction and damping discussed below the interface energy can take on a substantial positive value especially if there is, in the case of friction, substantial sliding. 29.8.5 Contact Damping Viscous contact damping has been added to all contact options including single surface contact. The original intent was to damp out oscillations normal to the contact surfaces during metal forming operations; however, it was later found to work effectively in removing high frequency noise in problems which involve impact. The input requires a damping value as a percentage of critical, 2𝑚, where 𝑚 is the mass and 𝜔 is the natural frequency. Letting 𝑘 denote the interface stiffness, we compute the natural frequency for an interface slave node from Equation 26.15. Contact-Impact Algorithm LS-DYNA Theory Manual Figure 29.17. Reaction forces with and without contact damping. 𝜔 = √ 𝑘(𝑚slave + 𝑚master) 𝑚slave𝑚master 𝑚 = min{𝑚slave, 𝑚master}. (29.24) The master mass 𝑚master is interpolated from the master nodes of the segment containing the slave node using the basis functions evaluated at the contact point of the slave node. Force oscillations often occur as curved surfaces undergo relative motion. In these cases contact damping will eliminate the high frequency content in the contact reaction forces but will be unable to damp the lower frequency oscillations caused by nodes moving from segment to segment when there is a large angle change between the segments. This is shown in the hemispherical punch deep drawing in Figure 29.16. The reaction forces with and without contact damping in Figure 29.17 show only minor differences since the oscillations are not due to the dynamic effects of explicit integration. However, refining the mesh as shown in Figure 29.18 to include more elements around the die corner as in Figure 29.18 greatly reduces the oscillations as shown in Figure 29.19. This shows the importance of using an adequate mesh density in applications where significant relative motion is expected around sharp corners. LS-DYNA Theory Manual Contact-Impact Algorithm Figure 29.18. Refinement of die radius. Friction Figure 29.19. The oscillations are effectively eliminated by the mesh refinement. Contact-Impact Algorithm LS-DYNA Theory Manual Friction in LS-DYNA is based on a Coulomb formulation. Let 𝐟∗ be the trial force, 𝐟𝑛 the normal force, 𝑘 the interface stiffness, 𝜇 the coefficient of friction, and 𝐟𝑛 the frictional force at time 𝑛. The frictional algorithm, outlined below, uses the equivalent of an elastic plastic spring. The steps are as follows: 1. Compute the yield force, 𝐹𝑦: 𝐹𝑦 = 𝜇 |𝐟𝑛| 2. Compute the incremental movement of the slave node 𝑛) 𝑛, 𝜂𝑐 Δ𝐞 = 𝐫𝑛+1(𝜉𝑐 𝑛+1) − 𝐫𝑛+1(𝜉𝑐 𝑛+1, 𝜂𝑐 3. Update the interface force to a trial value: 4. Check the yield condition: 𝐟∗ = 𝐟𝑛 − 𝑘Δ𝐞 𝐟𝑛+1 = 𝐟∗ if ∣𝐟∗∣ ≤ 𝐹𝑦 5. Scale the trial force if it is too large: 𝐟𝑛+1 = 𝐹𝑦𝐟∗ |𝐟∗| if ∣𝐟∗∣ > 𝐹𝑦 (29.25) (29.26) (29.27) (29.28) (29.29) An exponential interpolation function smooths the transition between the static, 𝜇𝑠, and dynamic, 𝜇𝑑, coefficients of friction where 𝐯 is the relative velocity between the slave node and the master segment: where 𝜇 = 𝜇𝑑 + (𝜇𝑠 − 𝜇𝑑) 𝑒−𝑐|𝐯|, 𝐯 = Δ𝐞 Δ𝑡 , Δ𝑡 is the time step size, and 𝑐 is a decay constant. (29.30) (29.31) The interface shear stress that develops as a result of Coulomb friction can be very large and in some cases may exceed the ability of the material to carry such a stress. We therefore allow another limit to be placed on the value of the tangential force: 𝑓 𝑛+1 = min(𝑓Coulomb 𝑛+1 , 𝜅𝐴master), (29.32) where 𝐴master is the area of the master segment and 𝜅 is the viscous coefficient. Since more than one node may contribute to the shear stress of a segment, we recognize that the stress may still in some cases exceed the limit 𝜅. Typical values of friction, see Table 26.1, can be found in Marks Engineering Handbook. LS-DYNA Theory Manual Contact-Impact Algorithm MATERIALS Hard steel on hard steel Mild steel on mild steel Aluminum on mild steel Aluminum on aluminum1 Tires on pavement (40psi) STATIC 0.78 (dry) 0.74 (dry) 0.61 (dry) 05 (dry) 0.90 (dry). SLIDING 08 (greasy), .42 (dry) 10 (greasy), .57 (dry) 47 (dry) 1.4 (dry) 69(wet), .85(dry) Table 26.1. Typical values of Coulomb Friction [Marks] 29.9 Tied Interfaces Sudden transitions in zoning are permitted with the tied interfaces as shown in Figure 29.20 where two meshes of solid elements are joined. This feature can often decrease the amount of effort required to generate meshes since it reduces the need to match nodes across interfaces of merged parts. Tied interfaces include four interface options of which three are in the Sliding Interface Definition Section in the LS-DYNA User’s Manual. These are: • Type 2 for tying surfaces with translational degrees of freedom. • Type 6 for tying translational degrees of freedom of nodes to a surface Figure 29.20. Tied interface used for a mesh transition. Tied interface permits mesh transitions Contact-Impact Algorithm LS-DYNA Theory Manual • Type 7 for tying both translational and rotational degrees of freedom of nodes The fourth option is in the “Tie-Breaking Shell Definitions” Section of the user’s manual and is meant as a way of tying edges of adjacent shells together. Unlike Type 7 this latter option does not require a surface definition, simply nodal lines, and includes a failure model based on plastic strain which can be turned off by setting the plastic failure strain to a high value. The first two options, which are equivalent in function but differ in the input definition, can be properly applied to nodes of elements which lack rotational degrees of freedom. The latter options must be used with element types that have rotational degrees of freedom defined at their nodes such as the shell and beam elements. One important application of Type 7 is that it allows edges of shells to be tied to shell surfaces. In such transitions the shell thickness is not considered. Exceptions from these latter statements is in case of invoking the implicit accuracy option, see *CONTROL_ACCURACY, for which a node with rotational degrees of freedom can tie to any element with or without offset. In this case moments are consistently transferred based on the kinematics of the chosen tied interface, the theory for this is presented in Section. Since the constraints are imposed only on the slave nodes, the more coarsely meshed side of the interface is recommended as the master surface. Ideally, each master node should coincide with a slave node to ensure complete displacement compatibility along the interface, but in practice this is often difficult if not impossible to achieve. In other words, master nodes that do not coincide with a slave node can interpenetrate through the slave surface. Implementation of tied interface constraints is straightforward. Each time step we loop through the tied interfaces and update each one independently. First, we distribute the nodal forces and nodal mass of each slave node to the master nodes which define the segment containing the contact point, i.e., the increments in mass and forces Δ𝑓𝑚 𝑖 = 𝜙𝑖(𝜉𝑐,𝜂𝑐)𝑓𝑠 (29.33) are added to the mass and force vector of the master surface. After the summation over all slave nodes is complete, we can compute the acceleration of the master surface. The acceleration of each slave node 𝑎𝑖𝑠 is then interpolated from the master segment containing its contact points: 𝑎𝑖𝑠 = ∑ 𝜙𝑗(𝜉𝑐, 𝜂𝑐)𝑎𝑖 . 𝑗=1 (29.34) Velocities and displacements are now updated normally. The interpolated contact point, (𝜉𝑐, 𝜂𝑐), for each slave node is computed once, since its relative position on the master segment is constant for the duration of the calculation. If the closest point projection of the slave node to the master surface is non- LS-DYNA Theory Manual Contact-Impact Algorithm orthogonal, values of (𝜉𝑐, 𝜂𝑐) greater than unity will be computed. To allow for slight errors in the mesh definition, the slave node is left unconstrained if the magnitude of the contact point exceeds 1.02. Great care should be exercised in setting up tied interfaces to ensure that the slave nodes are covered by master segments. Conflicting constraints must be avoided. Care should be taken not to include nodes that are involved in a tied interfaces in another tied interface, in constraint sets such as nodal constraint sets, in linear constraint equations, and in spot welds. Furthermore, tied interfaces between rigid and deformable bodies are not permitted. LS-DYNA checks for conflicting constraints on nodal points and if such conflicts are found, the calculation will terminate with an error message identifying the conflict. Nodes in tied interfaces should not be included as slave nodes in rigid wall definitions since interactions with stonewalls will cause the constraints that were applied in the tied interface logic to be violated. We do not currently check for this latter condition is LS-DYNA. Tied interfaces require coincident surfaces and for shell element this means that the mid-surfaces must be coincident. Consider Figure 29.21 where identical slave and master surfaces are offset. In this case the tied constraints require that translational velocities of tied nodes be identical, i.e., 𝐯𝑠 = 𝐯𝑚. (29.35) Consequently, if the nodes are offset, rotations are not possible. The velocity of a tied slave node in Figure 29.21 should account for the segment rotation: 𝐯𝑠 = 𝐯𝑚 − 𝑧̂ 𝐞3 × 𝛚, (29.36) where 𝑧̂ is the distance to the slave node, 𝐞3 is the normal vector to the master surface at the contact point, and 𝛚 is the angular velocity. Since this is not the case in the tied interfaces logic, 𝑧̂ must be of zero length. LS-DYNA projects tied slave nodes back to the master surface if possible and prints warning messages for all projected offset nodes or nodes too far away to tie. This projection eliminates the problems with rotational constraints but creates other difficulties: • Geometry is modified • Tied interfaces must be excluded from automatic generation since tied surfaces cannot be mixed with automatic contact with thickness offsets. Contact-Impact Algorithm LS-DYNA Theory Manual Slave Surface Master Surface Figure 29.21. Offset tied interface. An offset capability has been added to the tied interfaces which uses a penalty approach. The penalty approach removes the major limitations of the constraint formulation since with the offset option: • Multiple tied interfaces cannot share common nodes. • Rigid body nodes can be constrained. • Tied interface nodes can have other constraints applied and can be subjected to prescribed motions. 29.10 Strongly Objective Tied Contacts In implicit calculations, non-physical results observed when some tied contact formulations are combined with automatic single point constraints on solid element rotational degrees of freedom (AUTOSPC on *CONTROL_IMPLICIT_SOLVER) have motivated an extension in this context. A goal is to provide a universal tied contact formulation in implicit that works well in most situations, thus preventing the user from having to think too hard about which interface is best suited for the application at hand. To this end, a small selection of tied interfaces have been singled out that all represent this universal contact, these are *CONTACT_TIED_NODES_TO_SURFACE_CONSTRAINED_OFFSET *CONTACT_TIED_NODES_TO_SURFACE_OFFSET *CONTACT_TIED_SHELL_EDGE_TO_SURFACE_CONSTRAINED_OFFSET *CONTACT_TIED_SHELL_EDGE_TO_SURFACE_BEAM_OFFSET The first of these two do not consider rotational degrees of freedom, whereas the other two do. Furthermore, the first and third are constraint based and the other two are penalty based, so all in all these four cover much of what a user expects from a tied interface. By setting IACC to 1 on *CONTROL_ACCURACY any of the tied contact options mentioned above (and the non-offset counterparts as a side effect, i.e., *CONTACT_TIED_NODES_TO_SURFACE and *CONTACT_TIED_SHELL_EDGE_TO_SURFACE) are this strongly objective formulation. In addition to being strongly objective, i.e., forces and moments treated with LS-DYNA Theory Manual Contact-Impact Algorithm transform correctly under superposed rigid body motions in a single implicit step, this formulation applies rotational constraints consistently when and only when necessary. This means not only that slave nodes without rotational degrees of freedom are not rotationally constrained, but also that bending and torsional rotations are constrained to the master segment’s rotational motion in a way that is physically justified. To be more specific, slave node bending rotations (i.e., rotations in the plane of the master segment) are constrained to the master segment rotational degrees of freedom if this happens to stem from a shell element, otherwise they are constrained to the master segment rotation as determined from its individual nodal translations. The slave node torsional rotations (i.e., rotations with respect to the normal of the master segment) are always constrained according to this latter philosophy, thus avoiding a torsional constraint to the relatively weak drilling mode of shells. So this tied contact formulation properly treats bending and torsional rotations, here slave node rotational degrees of freedom typically come from shell or beam elements. So in effect, it is in a sense sufficient to only consider *CONTACT_TIED_SHELL_EDGE_TO_SURFACE_CONSTRAINED_OFFSET *CONTACT_TIED_SHELL_EDGE_TO_SURFACE_BEAM_OFFSET for most situations (choosing between a constraint or penalty formulation) but the other two *CONTACT_TIED_NODES_TO_SURFACE_CONSTRAINED_OFFSET *CONTACT_TIED_NODES_TO_SURFACE_OFFSET “non-rotational” formulations are included in the event of not wanting to constrain rotations whatsoever. Referring to Figure 2929-22, the following is the mathematical formulation of this tied contact formulation. Contact-Impact Algorithm LS-DYNA Theory Manual 𝑬0 𝛼𝜆 𝑭0 𝑮0 𝑠 𝑝 𝑚4 𝜆 𝑀 𝑡 = 0 𝑚2 𝑚1 𝑬 𝑭 Tying point 𝑚3 𝑡 > 0 Figure 2929-22 Kinematics of the implicit strong objective tied contact formulation 29.10.1 Kinematics We consider a slave node 𝑠 tied to a master segment 𝑀 with an offset 𝜆, the slave node projection onto the master segment is denoted 𝑝. Let 𝒙𝑠 denote the slave node coordinate and 𝒙𝑝 = ∑ ℎ𝑖𝒙𝑚 𝑖=1 (29.37) be the slave node projection on the master segment, where ℎ𝑖 are the constant isoparametric weights. To each of 𝑠, 𝑝 and 𝑀 we associate orthonormal bases (coordinate systems) represented by 𝑬 = {𝒆1 𝒆2 𝒆3} 𝑭 = {𝒇1 𝒇2 𝒇3} (29.38) (29.39) 𝒈2 𝒈3}, 𝑮 = {𝒈1 (29.40) respectively. The orthogonal matrix 𝑮 is the master segment coordinate system 𝑖 with normal 𝒈3. At 𝑡 = 0, we expressed as a function of the master coordinates 𝒙𝑚 initialize 𝑬0 = 𝑭0 = 𝑮0 but 𝑬 and 𝑭 then evolves independently based on the nodal rotational velocities 𝝎𝑠 and In the numerical implementation, if ∆𝜽𝑠 = 𝝎𝑠∆𝑡 and ∆𝜽𝑝 = 𝝎𝑝∆𝑡 are the incremental rotations of s and p at a given time step, then the coordinate systems are updated 𝝎𝑝 = ∑ ℎ𝑖𝝎𝑚 𝑖=1 . (29.41) LS-DYNA Theory Manual Contact-Impact Algorithm 𝑬𝑛+1 = 𝑹(∆𝜽𝑠)𝑬𝑛 (29.42) 𝑭𝑛+1 = 𝑹(∆𝜽𝑝)𝑭𝑛 (29.43) where 𝑹(∆𝜽) denotes the finite rotation matrix corresponding to the rotational increment ∆𝜽. Of course, this only makes sense if the slave node and/or master segment have rotational degrees of freedom. If the slave node lacks rotational degrees of freedom, then neither bending nor torsion is constrained and 𝑬 is of no interest. If on the other hand the master segment lacks rotational degrees of freedom, then we use 𝑭 = 𝑮 which is still of interest to deal with the offset, 𝑮 is always well-defined. LS-DYNA automatically detects rotational degrees of freedom and takes the proper measures. 29.10.2 Translational constraint Given the notation in the previous section and referring to Figure 2929-22, 𝒅 = {𝒙𝑠 − 𝛼𝜆𝒆3} − {𝒙𝑝 + (1 − 𝛼)𝜆𝒇3} (29.44) represents the vector we want to be zero in the translational part of the contact. Here 𝜆 is the offset distance between 𝑝 and 𝑠 and is constant throughout the simulation. Furthermore, 𝛼 is a constant between 0 and 1 that determines the actual tying point according to the following simple rules. First, if the slave node is connected to a solid or beam element or if the contact definition does not take rotational degrees of freedom into account, then 𝛼 = 0. Otherwise, if the slave node is connected to a shell element and the master segment is connected to a solid element, then 𝛼 = 1. If neither of those situations apply then both slave and master sides must connect to shell elements, for which 𝛼 = 0.5, so note that the value of 𝛼 is not accounting for the relative difference in shell thicknesses but assumes equal shell thickness on both master and slave sides. For and *CONTACT_TIED_NODES_TO_SURFACE_CONSTRAINED_OFFSET *CONTACT_TIED_SHELL_EDGE_TO_SURFACE_CONSTRAINED_OFFSET, this condition is imposed as a constraint for (29.45) and whereas *CONTACT_TIED_SHELL_EDGE_TO_SURFACE_BEAM_OFFSET penalty formulation is used. To this end we use a constitutive relation between force and displacement *CONTACT_TIED_NODES_TO_SURFACE_OFFSET 𝒅 = 𝟎 a (29.46) with 𝐾𝑓 as the penalty stiffness. Then an energy principle is employed to identify the nodal forces and moments, 𝒇 = 𝐾𝑓 𝒅 𝑇𝛿𝑿, (29.47) where 𝑿 is nodal coordinate array of the slave master pair, and 𝛿 is the variation operator. Identifying 𝑩𝑓 by 𝒇 𝑇𝛿𝒅 = 𝑷𝑓 𝛿𝒅 = 𝑩𝑓 𝛿𝑿 (29.48) the nodal force array is given by 𝑇𝒇 . (29.49) Worth noticing is that 𝑩𝑓 is the constraint matrix corresponding to the constraint variant of the contact. 𝑷𝑓 = 𝑩𝑓 Contact-Impact Algorithm LS-DYNA Theory Manual 29.10.3 Bending and torsion constraint If the slave node has rotational degrees of freedom and the contact formulation is said to treat those, bending and torsion is constrained. The bending strain is calculated as (29.50) which essentially is a measure of the amount 𝒆3 and 𝒇3 deviates from being parallel. The torsional strain is a scalar given by 𝜑𝑗 = 𝒈𝑗 𝑗 = 1,2 𝑇(𝒆3 × 𝒇3), 𝑇𝒈2 − 𝒆2 and is a measure of the relative rotation between 𝑬 and 𝑮 with respect to the normal 𝒈3. The constraint to enforce is 𝑇𝒈1) 𝜑3 = (29.51) (𝒆1 𝝋 = ⎜⎛ ⎝ 𝜑1 𝜑2 𝜑3⎠ ⎟⎞ = 𝟎 (29.52) which for a penalty formulation leads to a constitutive relation between moment and rotation vector (29.53) with 𝐾𝑚 being a stiffness parameter. Following the approach for translational treatment, we get the nodal force contribution 𝑇 𝒎 𝒎 = 𝐾𝑚𝝋 (29.54) 𝑷𝑚 = 𝑩𝑚 where Also here 𝑩𝑚 is the constraint matrix in case a constraint formulation is used. 𝛿𝝋 = 𝑩𝑚𝛿𝑿. (29.55) The formulae for 𝐾𝑓 and 𝐾𝑚 are found in earlier sections on tied interfaces while the expressions for the matrices 𝑩𝑓 and 𝑩𝑚 are quite involved and omitted for the sake of clarity, the nodal forces and moments are implemented by using (manual) algorithmic differentiation. 29.11 Sliding-Only Interfaces This option is seldom useful in structural calculations. Its chief usefulness is for treating interfaces where the gaseous detonation products of a high explosive act on a solid material. The present algorithm, though simple, has performed satisfactorily on a number of problems of this latter type. We briefly outline the approach here since the algorithm is still experimental and subject to change. The method consists of five steps. In the first step, the mass per unit area (mass/area) and pressure are found at each node on the slave surface. Next, the contact point for each master node is found, and the slave mass/area and slave pressure at each master node is interpolated from the slave surface. In the third step, this pressure distribution is applied to the master surface to update its acceleration. In the fourth step, the normal component of the acceleration at each node on the master surface is scaled by its z- LS-DYNA Theory Manual Contact-Impact Algorithm tied interface Figure 29.23. Incremental searching may fail on surfaces that are not simply connected. The new contact algorithm in LS-DYNA avoids incremental searching for nodal points that are not in contact and all these cases are considered. factor defined as the mass/area of the master surface at the master node divided by the sum of the mass/area of the slave surface at the master node. The last step consists of resetting the normal acceleration and velocity components of all slave nodes to ensure compatibility. 29.12 Bucket Sorting Bucket sorting is now used extensively in both the surface to surface and single surface contact algorithms. Version 920 of LS-DYNA no longer contains one-dimensional sorting. Presently two separate but similar bucket sorts are in LS-DYNA. In the first and older method we attempt to find for each node the three nearest nodes. In the newer method which is systematically replacing the older method we locate the nearest segment. The reasons for eliminating slave node tracking by incremental searching is illustrated in Figure 29.23 where surfaces are shown which cause the incremental searches to fail. In LS-DYNA tied interfaces are used extensively in many models creating what appears to the contact algorithms to be topologically disjoint regions. For robustness, our new algorithms account for such mesh transitions with only minor cost penalties. With bucket sorting incremental searches may still be used but for reliability they are used Contact-Impact Algorithm LS-DYNA Theory Manual Bucket Y Strips Figure 29.24. One- and two-dimensional bucket sorting. after contact is achieved. As contact is lost, the bucket sorting for the affected nodal points must resume. In a direct search of a set of 𝑁 nodes to determine the nearest node, the number of distance comparisons required is 𝑁 − 1. Since this comparison needs to be made for each node, the total number of comparisons is 𝑁(𝑁 − 1), with each of these comparisons requiring a distance calculation 12 = (𝑥𝑖 − 𝑥𝑗)2 + (𝑦𝑖 − 𝑦𝑗)2 + (𝑧𝑖 − 𝑧𝑗)2, (29.56) that uses eight mathematical operations. The cumulative effect of these mathematical operations for 𝑁(𝑁 − 1) compares can dominate the solution cost at less than 100 elements. The idea behind a bucket sort is to perform some grouping of the nodes so that the sort operation need only calculate the distance of the nodes in the nearest groups. Consider the partitioning of the one-dimensional domain shown in Figure 29.24. With this partitioning the nearest node will either reside in the same bucket or in one of the two adjoining buckets. The number of distance calculations is now given by LS-DYNA Theory Manual Contact-Impact Algorithm 3𝑁 − 1, (29.57) where 𝑎 is the number of buckets. The total number of distance comparisons for the entire one-dimensional surface is 𝑁 ( 3𝑁 − 1). (29.58) Thus, if the number of buckets is greater than 3, then the bucket sort will require fewer distance comparisons than a direct sort. It is easy to show that the corresponding number of distance comparisons for two-dimensional and three-dimensional bucket sorts are given by 𝑁 ( 9𝑁 𝑎𝑏 𝑁 ( 27𝑁 𝑎𝑏𝑐 − 1) for 2D − 1) for 3D (29.59) (29.60) where 𝑏 and 𝑐 are the number of partitions along the additional dimension. The cost of the grouping operations, needed to form the buckets, is nearly linear with the number of nodes 𝑁. For typical LS-DYNA applications, the bucket sort is 100 to 1000 times faster than the corresponding direct sort. However, the sort is still an expensive part of the contact algorithm, so that, to further minimize this cost, the sort is performed every ten or fifteen cycles and the nearest three nodes are stored. Typically, three to five percent of the calculational costs will be absorbed in the bucket sorting when most surface segments are included in the contact definition. 29.12.1 Bucket Sorting in TYPE 4 Single Surface Contact We set the number of buckets in the 𝑥, 𝑦, and 𝑧 coordinate directions to 𝑁𝑋, 𝑁𝑌, and 𝑁𝑍, respectively. Letting LMAX represent the longest characteristic length (found by checking the length of the segment diagonals and taking a fraction thereof) over all segments in the contact definition, the number of buckets in each direction is given by 𝑥max − 𝑥min LMAX 𝑁𝑋 = (29.61) , 𝑁𝑌 = 𝑦max − 𝑦min LMAX , (29.62) 𝑧max − 𝑧min LMAX where the coordinate pairs (𝑥min, 𝑥max), (𝑦min, 𝑦max), and (𝑧min, 𝑧max) define the extent of the contact surface and are updated each time the bucket searching is performed. In order to dynamically allocate memory effectively with FORTRAN, we further restrict 𝑁𝑍 = (29.63) , Contact-Impact Algorithm LS-DYNA Theory Manual the number of buckets such that the total number of buckets does not exceed the number of nodes in the contact surface, NSN or 5000: 𝑁𝑋 ⋅ 𝑁𝑌 ⋅ 𝑁𝑍 ≤ MIN (NSN, 5000). (29.64) If the characteristic length, LMAX, is large due to an oversized contact segment or an instability leading to a node flying off into space, the bucket sorting can be slowed down considerably since the number of buckets will be reduced. In older versions of DYNA3D this led to the error termination message “More than 1000 nodes in bucket.” The formulas given by Belytschko and Lin [1985] are used to find the bucket containing a node with coordinates (𝑥, 𝑦, 𝑧). The bucket pointers are given by 𝑃𝑋 = 𝑁𝑋 ⋅ (𝑥 − 𝑥min) (xmax − xmin) + 1, PY = NY ⋅ (𝑦 − 𝑦min) (𝑦max − 𝑦min) + 1, PZ = NZ ⋅ (𝑧 − 𝑧min) (𝑧max − 𝑧min) + 1, and are used to compute the bucket number given by NB = PX + (PY − 1) ⋅ PX + (PZ − 1) ⋅ PX ⋅ PY. (29.65) (29.66) (29.67) (29.68) For each nodal point, 𝑘, in the contact surface we locate the three nearest neighboring nodes by searching all nodes in buckets from MAX(1, PX1), MIN(NX, PX + 1), MAX(1, PY1), MIN(NY, PY + 1), MAX(1, PZ1), MIN(NZ, PZ + 1). (29.69) (29.70) (29.71) A maximum of twenty-seven buckets are searched. Nodes that share a contact segment with k are not considered in this nodal search. By storing the three nearest nodes and rechecking these stored nodes every cycle to see if the nearest node has changed, we avoid performing the bucket sorting every cycle. Typically, sorting every five to fifteen cycles is adequate. Implicit in this approach is the assumption that a node will contact just one surface. For this reason the single surface contact (TYPE 4 in LS-DYNA) is not applicable to all problems. For example, in metal forming applications both surfaces of the workpiece are often in contact. The nearest contact segment to a given node, 𝑘, is defined to be the first segment encountered when moving in a direction normal to the surface away from 𝑘. A major deficiency with the nearest node search is depicted in Figure 29.25 where the nearest nodes are not even members of the nearest contact segment. Obviously, this would not LS-DYNA Theory Manual Contact-Impact Algorithm be a problem for a more uniform mesh. To overcome this problem we have adopted segment based searching in both surface to surface and single surface contact. 29.12.2 Bucket Sorting in Surface to Surface and TYPE 13 Single Surface Contact The procedure is roughly the same as before except we no longer base the bucket size on 𝐿𝑀𝐴𝑋 which can result in as few as one bucket being generated. Rather, the product of the number of buckets in each direction always approaches 𝑁𝑆𝑁 or 5000 whichever is smaller, NX ⋅ NY ⋅ NZ ≤ MIN(NSN, 5000), (29.72) where the coordinate pairs (𝑥min, 𝑥max), (𝑦min, 𝑦max), and (𝑧min, 𝑧max) span the entire contact surface. In the new procedure we loop over the segments rather than the nodal points. For each segment we use a nested DO LOOP to loop through a subset of buckets from IMIN to IMAX, JMIN to JMAX, and to KMAX where IMIN = MIN(PX1, PX2, PX3, PX4), IMAX = MAX(PX1, PX2, PX3, PX4), JMIN = MIN(PY1, PY2, PY3, PY4), KMIN = MIN(PZ1, PZ2, PZ3, PZ4), KMAX = MAX(PZ1, PZ2, PZ3, PZ4), (29.73) (29.74) (29.75) (29.76) (29.77) and PX𝑘, PY𝑘, PZ𝑘 are the bucket pointers for the kth node. Figure 29.26 shows a segment passing through a volume that has been partitioned into buckets. We check the orthogonal distance of all nodes in the bucket subset from the segment. As each segment is processed, the minimum distance to a segment is determined for every node in the surface and the two nearest segments are stored. Therefore the required storage allocation is still deterministic. This would not be the case if we stored Normal vector at node 3 Figure 29.25. Nodes 2 and 4 share segments with node 3 and therefore the two nearest nodes are1 and 5. The nearest contact segment is not considered since its nodes are not members of the nearest node set. Contact-Impact Algorithm LS-DYNA Theory Manual Nodes in buckets shown are checked for contact with the segment Figure 29.26. The orthogonal distance of each slave node contained in the box from the segment is determined. The box is subdivided into sixty buckets. for each segment a list of nodes that could possibly contact the segment. We have now determined for each node, 𝑘, in the contact surface the two nearest segments for contact. Having located these segments we permanently store the node on these segments which is nearest to node 𝑘. When checking for interpenetrating nodes we check the segments surrounding the node including the nearest segment since during the steps between bucket searches it is likely that the nearest segment may change. It is possible to bypass nodes that are already in contact and save some computer time; however, if multiple contacts per node are admissible then bypassing the search may lead to unacceptable errors. 29.13 Single Surface Contact Algorithms in LS-DYNA The single surface contact algorithms evolved from the surface to surface contact algorithms and the post contact searching follows the procedures employed for the surface to surface contact. Type 4 contact in LS-DYNA uses the following steps where NSEG is the number of contact segments and NSN is the number of nodes in the interface: • Loop through the contact segments from 1 to NSEG ◦ Compute the normal segment vectors and accumulate an area weighted average at the nodal points to determine the normal vectors at the nodal points. LS-DYNA Theory Manual Contact-Impact Algorithm • Loop through the slave nodes from 1 to NSN ◦ Check all nearest nodes, stored from the bucket sort, and locate the node which is nearest. ◦ Check to see if nearest node is within a penetration tolerance determined during the bucket sort, if not, proceed to the end of the loop. ◦ For shell elements, determine if the nearest node is approaching the seg- ment from the positive or negative side based on the right hand rule. Pro- ject both the node and the contact segment along the nodal normal vectors to account for the shell thickness. ◦ Check for interpenetrating nodes and if a node has penetrated apply a nodal point force that is proportional to the penetration depth. End of Loop Of course, several obvious limitations of the above procedure exists. The normal vectors that are used to project the contact surface are meaningless for nodes along an intersection of two or more shell surfaces (Please see the sketch at the bottom of Figure 29.27). In this case the normal vector will be arbitrarily skewed depending on the choice of the numbering of the connectivities of the shells in the intersecting surfaces. Secondly, by considering the possibility of just one contact segment per node, metal forming problems cannot be handled within one contact definition. For example, if a workpiece is constrained between a die and a blankholder then at least some nodal points in the workpiece must necessarily be in contact with two segments-one in the die and the other in the workpiece. These two important limitations have motivated the development of the new bucket sorting procedure described above and the modified single surface contact procedure, type 13. A major change in type 13 contact from type 4 is the elimination of the normal nodal vector projection by using the segment normal vector as shown in Figure 29.27. Segment numbering within the contact surface is arbitrary when the segment normal is used greatly simplifying the model input generation. However, additional complexity is introduced since special handling of the nodal points is required at segment intersections where nodes may approach undetected as depicted in Figure 29.28a. To overcome this limitation an additional logic that put cylindrical cap at segment intersections has been introduced in contact type 13 (and a3). See Figure 29.28b. Assuming the segment based bucket sort has been completed and closest segments are known for all slave nodes then the procedure for processing the type 13 contact simplifies to: • Loop through the slave nodes from 1 to NSN Contact-Impact Algorithm LS-DYNA Theory Manual Type 4 Contact surface is based on a nodal point normal vector projection Type 13 Contact surface is based on segment normal projection Figure 29.27. Projection of the contact surface for a node approaching from above is shown for types 4 and 13 contact. ◦ If node is in contact, check to see if the contact segment has changed and if so, then update the closest segment information and the orientation flag which remembers the side in contact. Since no segment orientation infor- mation is stored this flag may change as the node moves from segment to segment. ◦ Check the closest segment to see if the node is in contact if not then pro- ceed to the end of the loop. If the slave node or contact segment connectiv- ity is a member of a shell element, project both the node and the contact segment along the segment normal vector to account for the shell thick- ness. A nodal thickness is stored for each node and a segment thickness is stored for each segment. A zero thickness is stored for solid elements. The thickness can be optionally updated to account for membrane thinning. ◦ Check for interpenetrating nodes and if a node has penetrated apply a nodal point force that is proportional to the penetration depth. End of Loop Note that type 13 contact does not require the calculation of nodal normal vectors. 29.14 Surface to Surface Constraint Algorithm The constraint algorithm that we implemented is based on the algorithm developed by Taylor and Flanagan [1989]. This involves a two-pass symmetric approach with a partitioning parameter, 𝛽, that is set between negative and positive unity where 𝛽 = 1 LS-DYNA Theory Manual Contact-Impact Algorithm Figure 29.28. and 𝛽 = −1 correspond to one way treatments with the master surface accumulating the mass and forces from the slave surface (for 𝛽 = 1) and visa versa (for 𝛽 = −1). The searching algorithms are those used in the other contact algorithms for the surface to surface contact. In this constraint approach the accelerations, velocities, and displacements are first updated to a trial configuration without accounting for interface interactions. After the update, a penetration force is computed for the slave node as a function of the penetration distance Δ𝐿: 𝐟𝑝 = 𝑚𝑠Δ𝐿 Δ𝑡2 𝐧, (29.78) where 𝐧 is the normal vector to the master surface. We desire that the response of the normal component of the slave node acceleration vector, 𝐚s, of a slave node residing on master segment 𝑘 be consistent with the motion of the master segment at its contact segment (𝑠c, 𝑡c), i.e., as = 𝜙1(𝑠c, 𝑡c)𝑎𝑛𝑘 1 + 𝜙2(𝑠c, 𝑡c)𝑎𝑛𝑘 2 + 𝜙3(𝑠c, 𝑡c)𝑎𝑛𝑘 3 + 𝜙4(𝑠c, 𝑡c)𝑎𝑛𝑘 4 . (29.79) For each slave node in contact with and penetrating through the master surface in its trial configuration, its nodal mass and its penetration force given by Equation (29.72) is accumulated to a global master surface mass and force vector: where (𝑚𝑘 + ∑ 𝑚𝑘𝑠 ) 𝐚𝑛𝑘 = ∑ 𝐟𝑘𝑠 , 𝑚𝑘𝑠 = 𝜙𝑘𝑚𝑠, 𝐟𝑘𝑠 = 𝜙𝑘𝐟𝑠. (29.80) (29.81) (29.82) Contact-Impact Algorithm LS-DYNA Theory Manual After solving Equation (29.78) for the acceleration vector, 𝐚nk, we can obtain the acceleration correction for the slave node as 𝐚ns = 𝐚s − 𝐟p 𝑚s . (29.83) The above process is repeated after reversing the master and slave definitions. In the final step the averaged final correction to the acceleration vector is found final = 𝐚𝑛 (1 − 𝛽)𝐚𝑛 1st pass + (1 + 𝛽)𝐚𝑛 2nd pass, and used to compute the final acceleration at time 𝑛 + 1 𝐚𝑛+1 = 𝐚trial + 𝐚𝑛 final, (29.84) (29.85) Friction, as described by Taylor and Flanagan [1989], is included in our implementation. Friction resists the relative tangential velocity of the slave node with respect to the master surface. This relative velocity if found by subtracting from the relative velocity: 𝐯r = 𝐯s − (𝜙1𝐯𝑘 1 + 𝜙2𝐯𝑘 2 + 𝜙3𝐯𝑘 3 + 𝜙4𝐯𝑘 4), the velocity component normal to the master segment: 𝐯t = 𝐯r − (𝐧 ⋅ 𝐯r)𝐧. A trial tangential force is computed that will cancel the tangential velocity 𝐟∗ = 𝑚𝑠𝜐𝑡 Δ𝑡 , where υt is the magnitude of the tangential velocity vector 𝜐𝑡 = √𝐯𝑡 ⋅ 𝐯𝑡. (29.86) (29.87) (29.88) (29.89) The magnitude of the tangential force is limited by the magnitude of the product of the Coulomb friction constant with the normal force defined as The limiting force is, therefore, And fn = ms𝐚ns ⋅ 𝐧, Fy = m|𝐟n|, 𝐟𝑛+1 = 𝐟∗ if 𝐟𝑛+1 = 𝐹𝑦𝐟∗ |𝐟∗| ∣𝐟∗∣ = 𝐹𝑦, if ∣𝐟∗∣ > 𝐹𝑦. (29.90) (29.91) (29.92) (29.93) LS-DYNA Theory Manual Contact-Impact Algorithm Therefore, using the above equations the modification to the tangential acceleration component of the slave node is given by 𝐚t = min (𝜇𝐚nt ⋅ 𝐧, ∣𝐯s∣ Δ𝑡 ), which must act in the direction of the tangential vector defined as 𝐧t = 𝐯t υt . The corrections to both the slave and master node acceleration components are: ats = at𝐧t, (29.94) (29.95) (29.96) asms mk The above process is again repeated after reversing the master and slave definitions. In the final step the averaged final correction to the acceleration vector is found 𝐚tk = −𝜙k (29.97) 𝐧t, final = 𝐚t (1 − 𝛽)𝐚t 1st pass + (1 + 𝛽)𝐚t 2nd pass, and is used to compute the final acceleration at time 𝑛 + 1 𝐚𝑛+1 = 𝐚trial + 𝐚𝑛 final + 𝐚t final. (29.98) (29.99) A significant disadvantage of the constraint method relative to the penalty method appears if an interface node is subjected to additional constraints such as spot welds, constraint equations, tied interfaces, and rigid bodies. Rigid bodies can often be used with this contact algorithm if their motions are prescribed as is the case in metal forming. For the more general cases involving rigid bodies, the above equations are not directly applicable since the local nodal masses of rigid body nodes are usually meaningless. Subjecting the two sides of a shell surface to this constraint algorithm will also lead to erroneous results since an interface node cannot be constrained to move simultaneously on two mutually independent surfaces. In the latter case the constraint technique could be used on one side and the penalty method on the other. The biggest advantage of the constraint algorithm is that interface nodes remain on or very close to the surfaces they are in contact with. Furthermore, elastic vibrations that can occur in penalty formulations are insignificant with the constraint technique. The problem related to finding good penalty constants for the contact are totally avoided by the latter approach. Having both methods available is possibly the best option of all. Contact-Impact Algorithm LS-DYNA Theory Manual 29.15 Planar Rigid Boundaries The rigid boundary represents the simplest contact problem and is therefore treated separately. As shown in Figure 29.29 the boundary is flat, finite or infinite in extent and is defined by an outward normal unit vector n with the origin of n at a corner point on the wall if the wall is finite or at an arbitrary point on the wall if the wall extends to infinity. The finite wall is rectangular with edges of length L and M. Unit vectors l and m lie along these edges. A subset of nodes is defined, usually boundary nodes of the calculational model, that are not allowed to penetrate. Let k represent one such n+1 be the position vector from the origin of n to k after locally boundary node and let rk updating the coordinates. Each time step prior to globally updating the velocities and accelerations we check k to ensure that the nodes lies within the wall by checking that both inequalities are satisfied: 𝑛+1 ⋅ 𝐥 ≤ 𝐿, 𝐫𝑘 𝑛+1 ⋅ 𝐦 ≤ 𝑀. 𝐫𝑘 (29.100) This test is skipped for the infinite rigid wall. Assuming that the inequality is satisfied, we then check the penetration condition to see if k is penetrating through the wall, 𝑛+1 ⋅ 𝐧 < 0, 𝐫𝑘 (29.101) and if so, the velocity and acceleration components normal to the wall are set to zero: 𝑛 − (𝐚𝑘old 𝑛 − (𝐯𝑘old 𝑛 = 𝐚𝑘old 𝐚𝑘new 𝑛 = 𝐯𝑘old 𝐯𝑘new ⋅ 𝐧)𝐧, ⋅ 𝐧)𝐧. (29.102) Here 𝐚𝑘 and 𝐯𝑘 are the nodal acceleration and velocity of node k, respectively. This procedure for stopping nodes represents a perfectly plastic impact resulting in an irreversible energy loss. The total energy dissipated is found by taking the difference between the total kinetic energy of all the nodal points slaved to the rigid wall before and after impact with the wall. This energy is computed and accumulated in LS-DYNA and is printed in the GLSTAT (global statistics) file. The tangential motion of the boundary node may be unconstrained, fully constrained, or subjected to Coulomb friction while it is in contact with the rigid boundary. LS-DYNA Theory Manual Contact-Impact Algorithm Origin, if extent of stonewall is finite Figure 29.29. Vector n is normal to the stonewall. An optional vector l can be defined such that 𝐦 = 𝐧 × 𝟏. The extent of the stonewall is limited by defining L and M. A zero value for either of these lengths indicates that the stonewall is infinite in that direction. Coulomb friction acts along a vector defined as: 𝐧𝑡 = 𝐯𝑘new 𝑛 √𝐯𝑘new 𝑛 ⋅ 𝐯𝑘new , (29.103) The magnitude of the tangential force which is applied to oppose the motion is given as 𝑓𝑡 = min ⎜⎜⎜⎛𝑚𝑠√𝐯𝑘new Δ𝑡 ⎝ ⋅ 𝐯𝑘new , 𝜇|𝐟𝑛| , ⎟⎟⎟⎞ ⎠ (29.104) i.e., the maximum value required to hold the node in the same relative position on the stonewall or the product of the coefficient of friction and the magnitude of the normal force whichever is less. In Equation (29.104), ms is the mass of the slave node and f𝑛 is the normal force. 29.16 Geometric Rigid Boundaries The numerical treatment of geometric rigid walls is somewhat similar to that for the finite planar rigid walls. The geometric rigid walls can be subjected to a prescribed translational motion along an arbitrarily oriented vector; however, rotational motion is not permitted. As the geometric surface moves and contacts the structure, external work is generated which is integrated and added to the overall energy balance. In addition to the external work, plastic work also is generated as nodes contact the wall Contact-Impact Algorithm LS-DYNA Theory Manual regular prism cylinder flat surface sphere Figure 29.30. Vector n determines the orientation of the generalized stonewalls. For the prescribed motion options the wall can be moved in the direction V as shown. and assume the walls normal velocity at the point of contact. Contact can occur with any of the surfaces which enclose the volume. Currently four geometric shapes are available including the rectangular prism, the cylinder, flat surface, and sphere. These are shown in Figure 29.30. 29.17 VDA/IGES Contact This cabability allows the user to read VDA/IGES surfaces directly into LS-DYNA for analysis as contact surfaces. No mesh generation is required, and the contact is performed against the analytic surface. LS-DYNA supports the VDA standard and an important subset of the IGES entities including: •#100 Circle arc •#102 Composite Curve •#106 Copious data •#110 Lines •#112 Parametric polynomial curve •#114 Parametric polynomial surface LS-DYNA Theory Manual Contact-Impact Algorithm •#116 Points •#126 NURBS Curves •#128 NURBS Surfaces •#142 Curve on Parametric Surface •#144 Trimmed Parametric Surfaces •#402 form 7-group •#406 form 15-associate name First, the user must specify which VDA/IGES surfaces, faces, and groups should be attached to each material. This is done primarily through a special input file. Faces, surfaces, and groups from several different VDA/IGES input files can be combined into groups that later can be refered to by a user specified alias. For example, suppose a simple sheetmetal forming problem is going to be run. The user might have an input file that looks like this: file punch.vda punch.bin { alias punch { grp001 } } file die.vda die.bin { alias part1 { fce001 sur002 } alias part2 { fce003 } } file die2.vda die2.bin { alias part3 { fce004 } } file holder.vda holder.bin { alias holder { sur001 sur002 } } alias die { part1 part2 part3 } end In this example, the user has specified that the punch will be made up of the group "grp001" from the file "punch.vda". The VDA file is converted to a binary file "punch.bin". If this simulation is ever rerun, the VDA input can be read directly from the binary file thereby significantly reducing startup time. The die in this example is made up of several surfaces and faces from 2 different VDA files. This format of input allows the user to combine any number of faces, surfaces, and groups from any number of VDA files to define a single part. This single part name is then referenced within the LS-DYNA input file. The contact algorithm works as follows. For the sake of simplicity, we will refer to one point as being slaved to a single part. Again, this part will in general be made up of several VDA surfaces and faces. First, the distance from the point to each VDA surface is computed and stored. For that surface which is nearest the point, several other parameters are stored such as the surface coordinates of the near point on the surface. Contact-Impact Algorithm LS-DYNA Theory Manual slave point (x, y, z) Figure 29.31. The geometry of the patch is a function of the parametric coordinates 𝑠 and 𝑡. Each time step of the calculation this information is updated. For the nearest surface the new near point is calculated. For all other surfaces the distance the point moves is subtracted from the distance to the surface. This continually gives a lower bound on the actual distance to each VDA surface. When this lower bound drops below the thickness of the point being tracked, the actual distance to the surface is recalculated. Actually, if the nearest surface is further away from the point than some distance, the near point on the surface is not tracked at all until the point comes close to some surface. These precautions result in the distance from the point to a surface having to be totally recomputed every few hundred timesteps, in exchange for not having to continually track the point on each surface. To track the point on the nearest surface, a 2D form of Newton's method is used. The vector function to be solved specifies that the displacement vector from the surface to the point should be parallel to the surface normal vector. The surface tangent vectors are computed with respect to each of the two surface patch parameters, and the dot product taken with the displacement vector. See Figure 29.31 and Equation (29.104). (𝐩 − 𝐪) ⋅ ∂𝐪 ∂s = 0 and (𝐩 − 𝐪) ⋅ ∂𝐪 ∂t = 0. (29.105) This vector equation is then solved using Newton's method as in Equation (1.106). 𝐪𝑖+1 = 𝐪𝑖 − (𝐅′)−1𝐅, (29.106) where LS-DYNA Theory Manual Contact-Impact Algorithm previous location new location new nearest point previous nearest point Figure 29.32. Newton iteration solves for the nearest point on the analytical surface. 𝐅(𝑠, 𝑡) = ⎜⎜⎜⎜⎜⎛(𝐩 − 𝐪) ⋅ (𝐩 − 𝐪) ⋅ ⎝ ⎟⎟⎟⎟⎟⎞ ∂𝐪 ∂𝑠 ∂𝐪 ∂𝑡 ⎠ . (29.107) The convergence is damped in the sense that the surface point is not allowed to jump completely outside of a surface patch in one iteration. If the iteration point tries to leave a patch, it is placed in the neighboring patch, but on the adjoining boundary. This prevents the point from moving merely continuous (i.e., when the surface has a crease in it). Iteration continues until the maximum number of allowed iterations is reached, or a convergence tolerance is met. The convergence tolerance (as measured in the surface patch parameters) varies from patch to patch, and is based on the size and shape of the patch. The convergence criterion is set for a patch to ensure that the actual surface point has converged (in the spatial parameters x, y, and z) to some tolerance. 29.18 Simulated Draw Beads The implementation of draw beads is based on elastic-plastic interface springs and nodes-to-surface contact. The area of the blank under the draw bead is taken as the master surface. The draw bead is defined by a consecutive list of nodes that lie along the draw bead. For straight draw beads only two nodes need to be defined, but for curved beads sufficient nodes must be used to define the curvature. The draw bead line is Contact-Impact Algorithm LS-DYNA Theory Manual integration points along drawbead line points 1, 2, 3, and 4 define drawbeads Figure 29.33. The drawbead contact provides a simple way of including drawbead behavior without the necessity of defining a finite element mesh for the drawbeads. Since the draw bead is straight, each bead is defined by only two nodes. discretized into points that become the slave nodes to the master surface. The spacing of the points is determined by LS-DYNA such that several points lie within each master segment. This is illustrated in Figure 29.32. The dense distribution of point leads to a smooth draw bead force distribution which helps avoid exciting the zero energy (hourglass) modes within the shell elements in the workpiece. A three-dimensional bucket search is used for the contact searching to locate each point within a segment of the master surface. The nodes defining the draw beads can be attached to rigid bodies by using the extra nodes for rigid body input option. When defining draw beads, care should be taken to limit the number of elements that are used in the master surface definition. If the entire blank is specified the CPU cost increases significantly and the memory requirements can become enormous. An automated draw bead box, which is defined by specifying the part ID for the workpiece and the node set ID for the draw bead, is available. The automated box option allows LS-DYNA determine the box dimensions. The size of this box is based on the extent of the blank and the largest element in the workpiece as shown if Figure 29.34. The input for the draw beads requires a load curve giving the force due to the bending and unbending of the blank as it moves through the draw bead. The load curve may also include the effect of friction. However, the coulomb friction coefficients must be set to zero if the frictional component is included in the load curve. If the sign of the load curve ID is positive the load curve gives the retaining force per unit draw bead length as a function of displacement, δ. If the sign is negative the load curve defines the LS-DYNA Theory Manual Contact-Impact Algorithm Figure 29.34. The draw bead box option automatically size the box around the draw bead. Any segments within the box are included as master segments in the contact definition. maximum retaining force versus the normalized position along the draw bead. This position varies from 0 (at the origin) to 1 (at the end) along the draw bead. See Figures 29.35 and 29.36. When friction is active the frictional force component normal to the bead in the plane of the work piece is computed. Frictional forces tangent to the bead are not allowed. The second load curve gives the normal force per unit draw bead length as a function of displacement, δ. This force is due to bending the blank into the draw bead as the binder closes on the die and represents a limiting value. The normal force begins to develop when the distance between the die and binder is less than the draw bead depth. As the binder and die close on the blank this force should diminish or reach a plateau. This load curve was originally added to stabilize the calculation. As the elements of the blank move under the draw bead, a plastic strain distribution develops through the shell thickness due to membrane stretching and bending. To account for this strain profile an optional load curve can be defined that gives the plastic strain versus the parametric coordinate through the shell thickness where the parametric coordinate is defined in the interval from –1 to 1. The value of the plastic strain at each through thickness integration point is interpolated from this curve. If the plastic strain at an integration point exceeds the value of the load curve at the time initialization occurs, the plastic strain at the point will remain unchanged. A scale factor that multiplies the shell thickness as the shell element moves under the draw bead can also be defined as a way of accounting for any thinning that may occur. Contact-Impact Algorithm LS-DYNA Theory Manual positive load curve ID Penetration distande, δ negative load curve ID Normalized draw bead length Figure 29.35. Draw bead contact model defines a resisting force as a function of draw bead displacement. 29.19 Edge to Edge Contact Edge to edge contact can be important in some simulations. For example, if a fan blade breaks away from the hub in a jet turbine contact with the trailing blade will likely be along the edges of the blades. Edge to edge contact requires a special treatment since the nodal points do not make contact with the master segment which is the basis of the conventional contact treatments. Currently all automatic type contact possess edge-to- edge capabilities and therefore contact type 22 is only useful with those contact that do not possess this capability. All contact using the segment-based formulation have edge to edge capabilities. LS-DYNA Theory Manual Contact-Impact Algorithm D, depth of draw bead F = Ffriction +Fbending Figure 29.36. Draw bead contact model defines a resisting force as a function of draw bead displacement. The basis of single edge contact is the proven single surface formulation and the input is identical. The definition is by material ID. Edge determination is automatic. It is also possible to use a manual definition by listing line segments. The single edge contact is type 22 in the structured input or *CONTACT_SINGLE_EDGE in the keyword input. Contact-Impact Algorithm LS-DYNA Theory Manual Figure 29.37. Contact between edges requires a special treatment since the nodes do not make contact. This contact only considers edge to edge contact of the type illustrated in Figure 29.38. Here the tangent vectors to the plane of the shell and normal to the edge must point to each other for contact to be considered. 29.20 Beam to Beam Contact In the beam to beam contact the contact surface is assumed to be the surface of a cylinder as shown in Figure 29.39. The diameter of the contact cylinder is set equal to tangent vectors in plane of shell Figure 29.38. Single edge contact considers contact between two edges whose normals point towards each other. the square root of the area of the smallest rectangle that contains the cross section to LS-DYNA Theory Manual Contact-Impact Algorithm avoid tracking the orientation of the beam within the contact algorithm. Contact is found by finding the intersection point between nearby beam elements and checking to see if their outer surfaces overlap as seen in Figure 29.40. If the surfaces overlap the contact force is computed and is applied to the nodal points of the interacting beam elements. Actual beam cross section Contact surface Figure 29.39. Beam contact surface approximation. intersection point where forces are applied Figure 29.40. The forces are applied at the intersection point. Contact-Impact Algorithm LS-DYNA Theory Manual 29.21 Mortar Contact The Mortar contact was originally implemented as a forming contact intended for stamping analysis but has since then evolved to become a general purpose contact algorithm for implicit time integration. The Mortar option is today available for automatic single- and surface-to-surface contacts with proper edge treatment, beam contact, and optional features include tie, tiebreak and interference. Contact is often the one feature that overturns the implicit performance, so to facilitate debugging of the Mortar contacts there is substantial information on penetrations written to the LS- DYNA message files. The Mortar contact is a penalty based segment-to-segment contact with finite element consistent coupling between the non-matching discretization of the two sliding surfaces and the implementation is based on Puso and Laursen [2004a,b]. This consistency, together with a differentiable penalty function for penetrating and sliding segments, assert the continuity and (relative) smoothness in contact forces that is appealing when running implicit analyses. The algorithm is primarily focusing on accuracy and robustness, and the involved calculations associated with this aim make it expensive enough to be first and foremost recommended for implicit analysis. There are numerous details in the implementation that simply cannot be explained without making the presentation incomprehensible, the intention here is to summarize the general concepts of the theory behind the implementation and draw upon this to make some general recommendations on usage. 29.21.1 Kinematics The Mortar contact is theoretically treated as a generalized finite element where each element in this context consists of a pair of contact segments. The friction model in the ns Ts Slave segment X3 X2 X1 Master Segment Figure 29.41. Illustration of Mortar segment to segment contact Mortar contact is a standard Coulomb friction law. Each of the two segments has its LS-DYNA Theory Manual Contact-Impact Algorithm iso-parametric representation inherited from the underlying finite element formulation, so the coordinates for the slave and master segments can be written 𝒙𝑠 = 𝑁𝑠 𝒙𝑚 = 𝑁𝑚 𝑖(𝜉 , 𝜂) {𝒙𝑖 + 𝑗 (𝜉 , 𝜂) {𝒙𝑗 + 𝑡𝑠𝒏𝑠} 𝑡𝑚𝒏𝑚}, (29.21.108) where summation over repeated indices is implicitly understood, i.e., over the nodes. We here also account that the contact surface may be offset from the mid-surface of e.g. shells, in the direction of the normal, 𝒏𝑠 and 𝒏𝑚, by half the thickness, 𝑡𝑠 and 𝑡𝑚. The kinematics for the contact element can be written as the penetration 𝑑 = 𝒏𝑠 𝑇(𝒙𝑠 − 𝒙̅𝑚), (29.21.109) where 𝒏𝑠 is the slave segment normal and 𝒙̅𝑚 is the projected point on the master segment along the slave segment normal. The element is only defined for the intersection between the slave and master segment and for points where 𝑑 > 0, this domain is denoted 𝛱 and is illustrated by gray in the Figure above. The sliding rate 𝒔̇ is similarly defined as 𝒔̇ = 𝑻𝑠 𝑇(𝒙̇𝑠 − 𝒙̅ ̇𝑚), where 𝑻𝑠 are two co-rotational basis vectors pertaining to the slave segment. 29.21.2 Constitutive relation The contact pressure is given by the constitutive law 𝜎n = 𝛼𝛽𝑠𝛽𝑚𝜀𝐾s𝑓 ( 𝜀𝑑𝑐 𝑠), (29.21.110) (29.21.111) where 𝛼 = stiffness scaling factor (SFS*SLSFAC) 𝐾s = stiffness modulus of slave segment 𝜀 = 0.03 𝑠 = characteristic length of slave segment 𝑑𝑐 𝛽𝑠 = stiffness scale factor of slave segment (=1 unless specifically stated) 𝛽𝑚 = stiffness scale factor of master segment (=1 unless specifically stated) and 𝑓 (𝑥) = ⎧ { { ⎨ { { ⎩ 𝑥2 cubic function that depends on IGAP 𝑥 < 𝑑max 2𝜀𝑑𝑐 𝑑max 2𝜀𝑑𝑐 𝑠 ≤ 𝑥 . (29.21.112) where 𝑑max is the maximum penetration to be given below. The Coulomb friction law is expressed in terms of the tangential contact stress Contact-Impact Algorithm LS-DYNA Theory Manual where 𝜇 is the friction coefficient and 𝝈𝑡 = 𝜇𝜎𝑛 |𝒔| 𝑔 ( |𝒔| 𝜇𝑑 ), (29.21.113) 𝑔(𝑥) = ⎧ {{ ⎨ {{ ⎩ 𝑥 ≤ 1 − 𝜀 1 − ( 1 + 𝜀 − 𝑥 ) 1 − 𝜀 < 𝑥 ≤ 1 + 𝜀 . (29.21.114) 1 + 𝜀 < 𝑥 The update of 𝒔 is done incrementally and is at the end of the step modified so that |𝒔| ≤ 𝜇𝑑(1 + 𝜀) (29.21.115) after the contact update. 29.21.3 Contact nodal forces From the contact stress, the contact nodal forces are determined by the principle of virtual work 𝑖 = 𝛿𝑖 𝒇𝑠 𝑘 {𝑰 + 𝑡𝑠 } {𝒏𝑠 ∫ 𝑁𝑠 𝑘𝜎𝑛𝑑𝛱 + 𝑻𝑠 ∫ 𝑁𝑠 𝑘𝝈𝑡𝑑𝛱 } (29.21.116) 𝑗 = 𝛿𝑗 𝒇𝑚 𝑘 {𝑰 + 𝑡𝑚 } {−𝒏𝑠 ∫ 𝑁𝑚 𝑘 𝜎𝑛𝑑𝛱 − 𝑻𝑠 ∫ 𝑁𝑚 𝑘 𝝈𝑡𝑑𝛱 }, 𝜕𝒏𝑠 𝜕𝒙𝑘 𝜕𝒏𝑚 𝜕𝒙𝑘 where the subscript 𝑠 and 𝑚 stands for the slave and master nodal forces, respectively, and 𝛿 denotes the Kronecker delta. Worth noting here is that accounting for offsets in the kinematic description leads to a term that will induce a torque due to frictional tractions. To this end, we need to remark that the kinematics for shell edges do not fall into the framework presented here; the actual map between the nodal and segment coordinates is not accounted for and contact traction will in those cases only induce translational forces on the nodes along the edge. For beams, nodal rotations are involved in the kinematics and frictional torques are accounted for but in a different way. 29.21.4 Treatment of beams, sharp solid and shell edges The automatic Mortar contacts support contact with the lateral surface and end tips of beams as well as edges of shell elements and sharp edges of solids. The concept of sharp solid edges will be defined below. The theory presented above is in this case applied to dummy segments corresponding to a faceted representation of the beam lateral surface and the edges of the solid and shell elements, respectively, as indicated in Figure 29-42. For a beam element the contact surface is represented by 14 faceted segments encapsulating a cylinder with the same length and volume as the beam element itself. This implies that all beam elements are assumed to have a circular cross section for the contact. The edges of the shell element surface are identified assuming the user contact definition (slave or master) consists of the entire physical component (metal sheet) in question. It is therefore recommended to •Define the contacts using part or part sets or otherwise false edges may be created in the interior of the component. LS-DYNA Theory Manual Contact-Impact Algorithm An edge contact element is created by extruding the shell edge in the direction of the shell normal by a distance corresponding to the shell thickness with appopriate adjustments for irregular geometries. As mentioned above, the kinematics in creating these edge segments do not account for its numerical representation and whence the Mortar contact does not assemble the corresponding forces in a finite element consistent manner. The shell edge treatment is to be seen as a simplified treatment just to incorporate a contact resistance for these geometries, which is probably ok in most practical situations. For beam elements however, rotational degrees of freedom are included in a consistent way, thus causing beam elements to rotate with respect to their axes when tangential friction forces are applied to the lateral surface. A sharp solid edge is detected when the angle 𝜃 between the normals of two adjacent contact segments is larger than 𝜋/3, and in this case the edge is smoothed by adding 4 segments between the two nodes common to the two contact segments, while at the same time adjusting the size of the two main contact segments. The effect is a rounded representation of the edge and a smoother contact response, see Figure 29-42. The size of the smoothing is at most 5% of the size of the smallest of the two contact segments, so the effect is reduced with mesh refinement. Since the contact area of these edge segments may be small, the stiffness of the contact is for those scaled by the factor 𝛽 = √3cot (𝜋−𝜃 2 ) where 𝜃 is the initial angle between the main segment normals. This scale factor is applied for both the slave and master side, meaning that if two right angled edges come into contact the 𝜋−𝜋 𝜋−𝜋 2 ) √3 cot ( stiffness is scaled by 𝛽𝑠𝛽𝑚 = √3 cot ( 2 ) = 9. Whether this is sufficient to handle most common situations is currently unknown, so this design decision is subject for change in the future. If a contact segment has two sharp edges with a common node, then a segment is created at the location of that node to account for contact with the corner of the solid element geometry. The stiffness scale factor for a corner node is the average of the scale factor for the connected edges. The motivation behind the solid edge smoothing is two-fold; for one thing it adds the feature of resisting penetration between a solid edge/corner and other geometries and then it also aids establishing a physical contact state when solid elements slide off sharp geometrical objects. More specifically it eliminates the ambiguity of which contact segments are in contact with which, and presumably prevents sudden spikes in the contact force, this is also illustrated in Figure 29-42. It is important to stress that the automatic Mortar contact surfaces are always located on the outer geometry for both slave and master sides, i.e., contact does not occur on the mid-surface of shells. A common modelling problem is illustrated in Figure 29-43 that results in extremely large contact stress unless the ignore flag is appropriately used. The forming contact is treated differently not only in that shell edge or beam contact is not supported. Here any shell master surface must be rigid with its segment normals oriented towards the slave side of the contact. Furthermore the contact occurs here on the mid-surface in contrast to the automatic option, while contact on the slave side still occurs on the outer geometry. The segment orientation of the (deformable) slave side is on one hand arbitrary, but if it consists of shell elements contact can only occur on one side for a given contact definition. In a forming application for instance, the contact Contact-Impact Algorithm LS-DYNA Theory Manual between the tool and blank and the contact between the die and blank have to be defined using two different contact interfaces since these contacts typically occur on different sides of the blank. Forming solid master surfaces may be rigid or deformable, thus allowing for effects of tool deformation and/or cooling effects. LS-DYNA Theory Manual Contact-Impact Algorithm Figure 29-42 29 Faceted representation of beams (including 4 quads representing a tip end), shell and sharp solid edges, respectively, the segment geometry indicated by red. The contact surface representation of three cubic solid elements is illustrated, with a somewhat exaggerated smoothing for illustration purposes. The effect of edge smoothing in contact is illustrated in a section cut bottom right, if the red objects slides to the right and the blue objects are fixed, the sudden detection of a parasitic contact indicated by the double arrow results in a jump in the contact force, this is alleviated by smoothing of the edges below. Contact-Impact Algorithm LS-DYNA Theory Manual Correct modelling if IGNORE is used, master edge shows excessive penetration but contact surface is adjusted Incorrect modelling if IGNORE is not used, master edge shows excessive penetration, large contact stress Correct modelling regardless of IGNORE, master edge is located on outer surface of slave segment, zero contact stress Figure 29-43 Intersected view of shells in edge-to-surface contact. Shell mid- surfaces indicated by dashed lines, outer surfaces by solid lines. Slave shell nodes are blue, master shell nodes are red and initial volume of penetration is shaded. 29.21.5 Characteristic length and contact release 𝑠 and 𝑑𝑐 𝑚 of the slave and master sides, respectively, are The characteristic lengths 𝑑𝑐 important in Mortar contact since they affect the contact stiffness but also because it determines the maximum allowed penetration between two arbitrary segments. To be more specific, two segments cannot penetrate more than 95% of the average characteristic lengths, penetrations larger than that will not be detected. In mathematical terms this can be stated as 𝑑max = 0.95 𝑠 + 𝑑𝑐 𝑑𝑐 (29.117) 𝑠 is the characteristic length of the slave where 𝑑max is the maximum penetration, 𝑑𝑐 𝑚 is the characteristic length of the master segment. This is illustrated in segment and 𝑑𝑐 Figure 29.44 that shows the contact stress as function of the relative penetration. To minimize the risk of releasing contacts one could increase the stiffness parameter SFS, but this may lead to worse convergence in implicit analysis. To this end, the IGAP parameter can be used to stiffen the contact for large penetrations without affecting moderate penetrations, this is also illustrated in Figure 29.44 and can be used if the contact pressure is locally very high. This also highlights the following important fact: The Mortar contact has no “stick” option for improving implicit convergence. LS-DYNA Theory Manual Contact-Impact Algorithm 4 3.5 3 2.5 2 1.5 1 0.5 0 0 IGAP=1 IGAP=2 IGAP=5 IGAP=10 0.2 0.4 0.6 0.8 1 Penetration Figure 29.44. Mortar contact stress as function of penetration relative 2𝑑max. This may on one hand lead to worse convergence characteristics but on the other rules out sticky behavior and underreport of contact forces in the ascii database. The characteristic length is for shells the shell thickness, whereas for solids it is a smaller element size in the part that the segment belongs to. The latter may lead to unrealistically high or low contact stiffness, or it may result in a too small maximum penetration depth, all depending on the mesh. For this reason the user may set PENMAX to the characteristic length, which should correspond to some physical member size in the model, and/or adjust the contact stiffness, depending on what the issue is. 29.21.6 Outputs for debugging implicit models In implicit analysis it is almost inevitable to run into convergence problems, especially when contacts are involved. When this happens the user usually craves for information on what’s gone wrong. For the Mortar contact, detailed information on penetration distance and potential contact release (i.e., penetration becomes too large for the contact to be detected in subsequent steps) can be requested through MINFO = 1 on CON- TROL_OUTPUT. With this option information on largest penetration, both absolute and relative, is given in the message files after each converged step, including a warning if penetration is close to being released. It also reports the elements with largest penetrations which makes it easy to locate critical areas of the model in LS-PrePost. Contact release should be avoided or otherwise results may be useless. On the other side of the spectrum, poor convergence could be due to a too stiff contact. Since the stiffness for a Mortar contact segment pair only depends on the slave segment it is recommended to Contact-Impact Algorithm LS-DYNA Theory Manual Contact surface augment SLDTHK Contact surface augment (SST × SFST-T)/2 Element thickness T Figure 29.45. Illustration of contact surface location for automatic Mortar contact, solids on top and shells below. •Put weak parts on the slave side If a steel part is in contact with rubber for instance, the rubber part should be put as slave side in the contact definition. One way of find contacts that cause poor convergence in implicit is to turn on D3ITCTL on CONTROL_IMPLICIT_SOLUTION and RESPLT on DATABASE_EXTENT_BINARY, which allows the user to isolate areas in the model where convergence is poor. Not rarely this is due to contacts. 29.21.7 Initial penetrations Initial penetrations are always reported in the message files, including the maximum penetration and how initial penetrations are to be handled. The IGNORE flag governs the latter and the options are IGNORE < 0 IGNORE = 0 IGNORE = 1 IGNORE = 2 IGNORE = 3 See explanation for the corresponding positive value, the only difference is that contact between segments belonging to the same part is not treated Initial penetrations will give rise to initial contact stresses, i.e., the slave contact surface is not modified, this option is not available for Mortar contact but defaults to IGNORE = 2 Initial penetrations will be tracked, i.e., the slave contact surface is translated to the level of the initial penetrations and subsequently follow the master contact surface on separation until the unmodified level is reached Initial penetrations will be ignored, i.e., the slave contact surface is translated to the level of the initial penetrations, optionally with an initial contact stress governed by MPAR1, this is the default option for Mortar contact Initial penetrations will be removed over time, i.e., the slave contact surface is translated to the level of the initial penetrations and pushed back to its unmodified level over a time determined by MPAR1 LS-DYNA Theory Manual Contact-Impact Algorithm IGNORE = 4 Same as IGNORE = 3 but it allows for large penetrations by also setting MPAR2 to at least the maximum initial penetration The use of IGNORE depends on the problem, if no initial penetrations are present there is no need to use this parameter at all. If penetrations are relatively small in relation to the maximum allowed penetration, then IGNORE = 1 or IGNORE = 2 seems to be the appropriate choice. For IGNORE = 2 the user may specify an initial contact stress small enough to not significantly affect the physics but large enough to eliminate rigid body modes and thus singularities in the stiffness matrix. The intention with this is to constrain loose parts that are initially close but not in contact by pushing out the contact surface using SLDTHK or SFST and applying the IGNORE = 2 option. Increasing SFST for shells to a number larger than unity will push the contact surface outside the geometry and contact will be detected accordingly, see Figure, the SLDTHK parameter is used for solids. It is at least good for debugging problems with many singular rigid body modes. IGNORE = 3 is the Mortar interference counterpart, used for instance if there is a desire to fit a rubber component in a structure or for eliminating initial penetrations by simulation. With this option the contact surfaces are restored linearly in time from the beginning of the simulation to the time specified by MPAR1. If the intention is to initial penetrations completely, and since contact penetrations are eliminate unavoidable to some extent, it may also in this case be of importance to use SFST or SLDTHK to reduce the possibility that the actual geometry is penetrated. If using a single surface definition on a complicated geometry with many parts, a negative value of IGNORE could be of interest, since the Mortar contact may otherwise detect spurious contacts between segments belonging to the same part. A drawback with IGNORE = 3 is that initial penetration must be smaller than half the characteristic length of the contact or otherwise they will not be detected in the first place. For this reason IGNORE = 4 was introduced where initial penetrations may be of arbitrary size, but it requires that the user provides crude information on the level of penetration of the contact interface. This is done in MPAR2 which must be larger than the maximum penetration or otherwise an error termination will occur. IGNORE = 4 only applies to solid elements at the moment. Contact-Impact Algorithm LS-DYNA Theory Manual 𝑠1 𝑠2 𝑚2 𝑚1 𝑠1 vs 𝑚2 𝒙1 𝑠1 vs 𝑚1 𝑑(𝑡) 𝒏𝑠 𝒚1 𝒙(𝑡) 𝒙2 𝒚(𝑡) 𝒏𝑚 𝒕 𝒚2 𝑠2 vs 𝑚2 29-4629 2D mortar contact, 2 slave segments in contact with 2 master segments results in three separate treatments. 29.21.8 2D Mortar contact Automatic single and surface-to-surface Mortar contact is available and here described in detail as an attempt to illustrate it in a setting that is hopefully easier to understand. In Figure 29-46 (top) the contact between 2 slave and 2 master segments is shown as an example. This particular configuration results in the treatment of 3 slave vs master contact pairs (bottom), and for the mathematical treatment we refer to this figure as an illustration. Kinematics First a common tangential direction is determined, this is given as 𝒕 = 𝒙2 + 𝒚2 − 𝒙1 − 𝒚1 ∥𝒙2 + 𝒚2 − 𝒙1 − 𝒚1∥ (29.118) and the corresponding normal 𝒏 is perpendicular to 𝒕, with the direction convention as illustrated. We can define a coordinate 𝑡 along this tangential direction, the origin can be chosen arbitrarily, and then 𝒙(𝑡) and 𝒚(𝑡) are the projection coordinate along 𝒏 onto the slave and master segment, respectively. Obviously there is a finite interval 𝑡 ∈ LS-DYNA Theory Manual Contact-Impact Algorithm [𝑡 ̃1, 𝑡 ̃2] where both 𝒙(𝑡) and 𝒚(𝑡) is well-defined, and on this interval we can define the penetration as 𝑑(𝑡) = 𝒏𝑇(𝒙(𝑡) − 𝒚(𝑡)). (29.119) The overlapped interval is then further reduced to 𝑡 ∈ [𝑡1, 𝑡2] for which 𝑑(𝑡) ≥ 0, note that for the 𝑠2 vs 𝑚2 situation these two intervals are not the same. The interval [𝑡1, 𝑡2] is indicated by red in the illustration. This completes the kinematics in the normal direction. In the tangential direction we need to define the kinematics for sliding and we do this by associating a history variable to each slave segment. To this end, 𝑆 as a weighted measure of the distance a slave segment has slid along the master surface and is defined as 𝑆 = 𝑆𝑛−1 + ∑ ∫ {𝑠(𝑡) − 𝒕𝑛−1 𝐴𝑖 𝑇 (𝒙𝑛−1(𝑡) − 𝒚𝑛−1(𝑡))}𝑑𝐴𝑖 (29.120) where 𝑠(𝑡) = 𝒕𝑇(𝒙(𝑡) − 𝒚(𝑡)) and the subscript 𝑛 − 1 refers to the corresponding value in the previous step. The integral is taken over the domain 𝐴𝑖 of the intersected interval between the slave segment and master segment 𝑖, accounting for plane strain or axial symmetry. Note that the slave segment can be in contact with several master segments, whence the sum. Further noting that by construction the first term in the integrand, 𝑠(𝑡) = 0, we can simplify this to 𝑆 = 𝑆𝑛−1 − ∑ ∫ 𝒕𝑛−1 𝑇 (𝒙𝑛−1(𝑡) − 𝒚𝑛−1(𝑡))𝑑𝐴𝑖 𝐴𝑖 . (29.121) In the illustrated situation, slave segment 1 would get sliding contributions from master segments 1 and 2, while slave segment 2 only from master segment 2. Likewise we define a weighted penetration which is used together with 𝑆 to define the friction law below. 𝐷 = ∑ ∫ 𝑑(𝑡)𝑑𝐴𝑖 𝐴𝑖 . (29.122) Constitutive relations For simplicity, we drop the explicit dependence on 𝑡 from now on and define the contact stress (pressure) as where 𝐾 is the contact stiffness defined as 𝜎𝑛 = 𝐾 𝑑2 𝐾 = 0.01 𝑇𝑠𝑇𝑚 2𝐾𝑠𝐾𝑚 𝐾𝑠 + 𝐾𝑚 𝑓 (𝒏𝑠 𝑇𝒏𝑚). (29.123) (29.124) Furthermore, 𝛼 = PSF ∗ SLSFAC is a stiffness scale factor and 𝑇𝑠/𝑚 and 𝐾𝑠/𝑚 are characteristic lengths and material stiffnesses of the slave and master segments, respectively. The function 𝑓 is used to linearly reduce stiffness for segments that are not parallel, note that 𝒏𝑠 and 𝒏𝑚 are the normals to the slave and master segments, and is given as Contact-Impact Algorithm LS-DYNA Theory Manual ⎧ { { { { { ⎨ { { { { { ⎩ The friction stress is defined as 𝑓 (𝑥) = − ≤ 𝑥 1 + 2𝑥 1 − √3 − √3 ≤ 𝑥 < − . 𝑥 < − √3 (29.125) 𝜇𝐷 with 𝜇 being the Coulomb friction coefficient and 𝑔 is a continuously differentiable function defined as 𝜎𝑡 = 𝜇𝜎𝑛𝑔 ( (29.126) ) 𝑔(𝑥) = ⎧ {{{{{ {{{{{ ⎨ ⎩ 1 − 25 1, 𝑥 ≥ 1.03 (𝑥 − 1.03)2, 0.97 ≥ 𝑥 > 1.03 𝑥, −0.97 ≥ 𝑥 > 0.97 −1 + 25 (𝑥 + 1.03)2, −1.03 ≥ 𝑥 > −0.97 −1, −1.03 > 𝑥 (29.127) The interpretation of this law is that the magnitude of friction stress 𝜎𝑡 is at most 𝜇𝜎𝑛, and the fraction thereof is determined by the appropriate relation between the accumulated sliding and penetration. Upon convergence, to yield a proper friction behavior, 𝑆𝑛 = the updated max (−1.03𝜇𝐷, min(1.03𝜇𝐷, 𝑆)). according next step for to is 𝑆 Nodal forces The nodal force contribution from a given segment pair is determined from the principle of virtual work, i.e., 𝛿𝑊 = ∫ 𝜎𝑛 𝛿𝑑 𝑑𝐴 . + ∫ 𝜎𝑡 𝛿𝑠 𝑑𝐴 (29.128) Here 𝛿 is the variation operator, and the independent variables subject to this variation are the nodal coordinates. Thus, replacing the left hand side with the expression involving nodal forces and coordinates, and using (29.123) and (29.126) for the right hand side we get ∑ 𝒇𝐼 𝑇𝛿𝒙𝐼 = 𝐾 ∫ 𝑑2 𝛿𝑑 𝑑𝐴 + 𝜇𝐾𝑔 ∫ 𝑑2 𝛿𝑠 𝑑𝐴 . The nodal forces are then readily identified as 𝒇𝐼 = 𝐾 ∫ 𝑑2 𝜕𝑑 𝜕𝒙𝐼 𝑑𝐴 + 𝜇𝐾𝑔 ∫ 𝑑2 𝜕𝑠 𝜕𝒙𝐼 . 𝑑𝐴 (29.129) (29.130) where the exact expressions for the integrals in terms the nodal coordinates are, although straightforward to derive, a bit lengthy and therefore omitted. Stiffness matrix LS-DYNA Theory Manual Contact-Impact Algorithm The stiffness matrix is the second variation of the virtual work expression (29.128) where we neglect the variation of the overlapped area and assume the variation can be taken on the integrand directly ∆𝛿𝑊𝐼 = 2𝐾 ∫ 𝑑 ∆𝑑 𝛿𝑑 𝑑𝐴 𝜇𝐷 𝜕𝑔 𝜕𝑥 + 𝜇 { + 2𝜇𝐾𝑔 ∫ 𝑑 ∆𝑑 𝛿𝑠 𝑑𝐴 ∆𝑆 − . 𝜇𝐷2 ∆𝐷} ∫ 𝜎𝑛 𝛿𝑠 𝑑𝐴 (29.131) Here ∆ is again the variation operator, different notation to distinguish it from 𝛿 but performing the exact same thing. At this point we emphasize that the (geometric) terms involving ∆𝛿𝑑 and ∆𝛿𝑠 have been deliberately excluded as they, albeit being symmetric, contribute to the indefiniteness of the tangent matrix. In (29.131), the first term on the right hand side is the normal-normal interaction and is nicely symmetric, the remaining terms come from friction (normal-tangent and tangent-tangent interaction) and needs symmetrization and further simplification. To this end we neglect any terms involving ∆𝑑 𝛿𝑠 and ∆𝐷𝛿𝑠 which means that it remains to deal with the term involving ∆𝑆 𝛿𝑠. The simplifications made are to approximate ∫ 𝜎𝑛 𝑑𝐴 in the last integral, and then neglect all terms in ∆𝑆 that do not pertain to the present slave master segment pair. This results in 𝜎𝑛 ≈ (29.132) ∆𝒙𝐼 𝑇𝑲𝐼𝐽 𝑇𝛿𝒙𝐽 ≈ 2𝐾 ∫ 𝑑 ∆𝑑 𝛿𝑑 𝑑𝐴 and the stiffness matrix can be identified as 𝜕𝑔 𝜕𝑥 + { ∫ 𝜎𝑛 𝑑𝐴 } {∫ ∆𝑠 𝑑𝐴 } {∫ 𝛿𝑠 𝑑𝐴 } (29.133) 𝑲𝐼𝐽 = 2𝐾 ∫ 𝑑 𝜕𝑑 𝜕𝒙𝐼 𝜕𝑑 𝜕𝒙𝐽 𝑑𝐴 + 𝜕𝑔 𝜕𝑥 { ∫ 𝜎𝑛 𝑑𝐴 } {∫ 𝜕𝑠 𝜕𝒙𝐼 𝑑𝐴 } {∫ 𝜕𝑠 𝜕𝒙𝐽 𝑑𝐴 }. (29.134) A characteristic feature of the Mortar contact, which can be deduced from this expression, is that not only the nodal forces are continuous but also the stiffness matrix. This follows from the 𝐶1 continuity of 𝑔, meaning that all involved functions above are continuous, and that 𝑲𝐼𝐽 tends to zero as either 𝑑 or 𝐴 tends to zero. A mathematical treatment yields ∥𝑲𝐼𝐽∥ ≤ 𝐾𝐴 max 𝑑(𝑡) {2 max 𝜕𝑑(𝑡) ∥ 𝜕𝒙𝐼 ∥ ∥ 𝜕𝑑(𝑡) 𝜕𝒙𝐽 ∥ + max ∥ 𝜕𝑠(𝑡) 𝜕𝒙𝐼 ∥ ∥ 𝜕𝑠(𝑡) 𝜕𝒙𝐽 ∥} (29.135) which tends to zero as 𝑑 or 𝐴 tends to zero as the terms inside the right bracket are bounded. 29.21.9 Tied and tiebreak option A tied and tiebreak option with the Mortar contact is available by appending MORTAR_TIED or TIEBREAK_MORTAR to the automatic surface to surface contact keyword. In principle, the tiebreak allows for specifying the contact stress 𝜎 as a function of the separation 𝑑 to accomodate a given interface law that includes softening and failure (loss of interface stiffness). The law incorporates both normal and tangential directions, usually denoted mode I and mode II in the delamination community, and the typical appearance of such a law is shown in Figure bm_figcohlaw. The law is in Contact-Impact Algorithm LS-DYNA Theory Manual general characterized by the energy release rate 𝐸 which is the energy per unit area required to release the contact, and the maximum interface stress 𝜎𝑒 which is the peak contact stress before softening begins. Referring to the above mentioned figure, the energy release rate is the integral of the curve describing the stress vs displacement relation. The law can indeed be quite complicated, and we refer to the keyword manual for more information regarding details of the cohesive models available. For the Mortar tiebreak option only OPTION = 7 and OPTION = 9 are supported. The internal treatment of the Mortar tied and tiebreak options are very similar to that of the one-sided contacts, but the following remarks are in place. •Tied Mortar contact is penalty based and exhibits a linear relationship between normal/tangential separation and resulting contact stress. In referring to equa- tion (29.21.111), 𝑓 (𝑥) = 𝑥 for all 𝑥 in all separation directions. Since the nonlineari- ty is significantly reduced compared to one-sided contacts, the implicit convergence characteristics are insensitive to scaling of the contact stiffness. •Tiebreak Mortar contact is treated similarly but the normal and tangential contact stress is given by the constitutive model. It is strongly recommended to set CN (OPTION = 7 and OPTION = 9) and CT2CN (only OPTION = 9) on the addition- al card associated with the tiebreak option, otherwise the interface stiffness is determined internally and may be inconveniently large. •Tiebreak Mortar contact is superposed by a one-sided contact to take compressive contact stress, mainly to prevent penetrations in the post-failure regime but also to prevent cohesive failure due to normal compression. This contact follows the theory described above and automatically applies the IGNORE = 2 option to start with an initial zero contact stress. •The one-sided contact associated with the tiebreak option is frictionless as long as the tied contact exists, this to avoid spurious interactions between the laws (mode II and friction) in the tangential directions. The friction is activated as soon as the tied contact is released. Furthermore, the tied interface will not take compressive stress as this is lent to the one-sided contact. •Tied and tiebreak Mortar contacts are applied if the initial normal distance between the slave and master segment (with respect to their outer geometries) is less than a critical distance, 𝑑𝑡 = 0.05𝑑𝑐. In this formula 𝑑𝑐 is the characteristic length as described above. Here 𝑑𝑡 =PENMAX can be used to override this tolerance for when to tie two segments, so the meaning of PENMAX is in this case different than for the unilateral contacts. LS-DYNA Theory Manual Contact-Impact Algorithm Shear Contact Forces Workpiece Support 150000 100000 50000 0 -50000 -100000 -150000 0 10 20 30 40 50 60 Workpiece Displacement Figure 29-47 A rubber compression example solved in implicit with Mortar contact (Courtesy of Dellner Couplers AB). The graph shows the contact force between the rubber parts and the moving workpiece and between the rubber parts and the two supports, respectively. LS-DYNA Theory Manual Geometric Contact Entities 30 Geometric Contact Entities Contact algorithms in LS-DYNA currently can treat any arbitrarily shaped surface by representing the surface with a faceted mesh. Occupant modeling can be treated this way by using fine meshes to represent the head or knees. The generality of the faceted mesh contact suffers drawbacks when modeling occupants, however, due to storage requirements, computing costs, and mesh generation times. The geometric contact entities were added as an alternate method to model cases of curved rigid bodies impacting deformable surfaces. Much less storage is required and the computational cost decreases dramatically when compared to the more general contact. Geometric contact entities are developed using a standard solids modeling approach. The geometric entity is defined by a scalar function 𝐺(𝑥, 𝑦, 𝑧). The solid is determined from the scalar function as follows: 𝐺(𝑥, 𝑦, 𝑧) > 0 The point (𝑥, 𝑦, 𝑧) is outside the solid 𝐺(𝑥, 𝑦, 𝑧) = 0 The point (𝑥, 𝑦, 𝑧) is on the surface of the solid 𝐺(𝑥, 𝑦, 𝑧) < 0 The point (𝑥, 𝑦, 𝑧) is inside the solid (30.1) (30.2) (30.3) Thus, by a simple function evaluation, a node can be immediately determined to be outside the solid or in contact. Figure 30.1 illustrates this for a cylinder. If the node is in contact with the solid, a restoring force must be applied to eliminate further penetration. A number of methods are available to do this such as Lagrange multipliers or momentum based methods. The penalty method was selected because it is the simplest and most efficient method. Also, in our applications the impact velocities are at a level where the penalty methods provide almost the identical answer as the exact solution. Using the penalty method, the restoring force is proportional to the penetration distance into the solid and acts in the direction normal to the surface of the solid. Thus, Geometric Contact Entities LS-DYNA Theory Manual G(x, y) < 0 G(x, y) > 0 G(x, y) = 0 Figure 30.1. Determination of whether a node is interior or exterior to the cylindrical surface the penetration distance and the normal vector must be determined. The surface normal vector is conveniently determined from the gradient of the scalar function. 𝐍(𝑥, 𝑦, 𝑧) = ∂𝐺 ∂𝑥 𝐢 + ∂𝐺 ∂𝑦 𝐣 + 𝜕𝐺 𝜕𝑧 , √(∂𝐺 ) ∂𝑥 + (∂𝐺 ) ∂𝑦 + (∂𝐺 ∂𝑧 ) (30.4) for all (𝑥, 𝑦, 𝑧) such that 𝐺(𝑥, 𝑦, 𝑧) = 0. The definition of 𝐺(𝑥, 𝑦, 𝑧) guarantees that this vector faces in the outward direction. When penetration does occur, the function 𝐺(𝑥, 𝑦, 𝑧) will be slightly less than zero. For curved surfaces this will result in some errors in calculating the normal vector, because it is not evaluated exactly at the surface. In an implicit code, this would be important, however, the explicit time integration scheme in DYNA3D uses such a small time step that penetrations are negligible and the normal function can be evaluated directly at the slave node ignoring any penetration. 𝐺(𝑥, 𝑦) = 𝑥2 + 𝑦2 − 𝑅2, (30.5) The penetrations distance is the last item to be calculated. In general, the penetration distance, 𝑑, is determined by. where 𝐗𝑛 is the location of node 𝑛 and 𝐗′𝑛 is the nearest point on the surface of the solid. 𝑑 = ∣𝐗𝑛 − 𝐗′𝑛∣, (30.6) To determine 𝐗′𝑛, a line function is defined which passes through 𝐗𝑛 and is normal to the surface of the solid: Substituting the line function into the definition of the Equation (30.2) surface of a solid body gives: 𝐋(𝑠) = 𝐗𝑛 + 𝑠𝐍 (𝐗𝑛). (30.7) LS-DYNA Theory Manual Geometric Contact Entities 𝐺(𝐗𝑛 + 𝑠𝐍(𝐗)) = 0. (30.8) If Equation (30.8) has only one solution, this provides the parametric coordinates s which locates 𝐗′𝑛. If Equation (30.8) has more than one root, then the root which minimizes Equation (30.6) locates the point 𝐗′𝑛. The penalty method defines the restoring forces as: 𝐟 = 𝑝𝑑𝐍(𝐗′̅̅̅̅̅̅̅ 𝑛), (30.9) where 𝑝 is a penalty factor and is effectively a spring constant. To minimize the penetration of the slave node into the solid, the constant 𝑝 is set large, however, it should not be set so large that the Courant stability criteria is violated. This criteria for the slave node tells us that: Δ𝑡 ≤ 𝜔max = = 2√ 𝑚𝑛 𝐾𝑛 , √𝐾𝑛 𝑚𝑛 (30.10) where 𝐾𝑛 is the stiffness of node 𝑛 and 𝑚𝑛 is the mass of node 𝑛. The penalty factor, 𝑝, is determined by choosing a value which results in a penalty/slave mass oscillator which has a characteristic time step that is ten times larger than the Courant time step: Solving for 𝑝𝑛 gives: 10Δ𝑡 = 2√ 𝑚𝑛 𝑝𝑛 . 𝑝𝑛 = 4𝑚𝑛 (100Δ𝑡2) . (30.11) (30.12) Inclusion of any structural elements into the occupant model will typically result in very large stiffnesses due to the small time step and the (1/Δ𝑡)2 term. Thus the method is highly effective even with impact velocities on the order of 1km/sec. The scalar function 𝐺(𝐗) is frequently more conveniently expressed as 𝑔(𝐱)where, 𝑔 is the function defined in local coordinates and 𝐱 is the position in local coordinates. The local entity is related to the global coordinates by: 𝐱 = [T](𝐗𝑗 − 𝐐𝑗), (30.13) where 𝐐𝑗 is the offset and [T] is a rotation matrix. The solid scalar function and the penetration distance can be evaluated in either local or global coordinates with no difference to the results. When working in local coordinates, the gradient of the local scalar function provides a normal vector which is in the local system and must be transformed into the global by: Geometric Contact Entities LS-DYNA Theory Manual An ellipsoid is defined by the function: 𝐍(𝐗̅̅̅̅̅) = [T]T𝐧(𝐱). 𝐺(𝑥, 𝑦, 𝑧) = ( ) + ( ) + ( ) − 1. The gradient of 𝐺 is 2𝑥 𝑎2 𝐢 + 2𝑦 𝑎2 𝐣 + 2𝑧 𝐧(𝑥, 𝑦, 𝑧) = 𝑎2 𝐤 and the normal vector is: 𝑏 2 𝐣 + 𝑧 𝑐 2 𝐤) 𝑦 2 𝑏 4 + 𝑧 2 ( 𝑥 𝑎 2 𝐢 + √𝑥 2 𝑎 4 + 𝑐 4 , Substituting Equations (30.7) and (30.15) into Equation (27.2) gives: [( 𝑛𝑥 𝑎 ) + ( 𝑛𝑦 𝑏 ) + ( + [( 𝑛𝑧 𝑐 ) 𝑥𝑛 ] 𝑠 2 + 2 [ ) + ( ) 𝑦𝑛 𝑛𝑥𝑥𝑛 𝑎 2 + 𝑧𝑛 + ( ) 𝑛𝑦𝑦𝑛 𝑏 2 + 𝑛𝑧𝑧𝑛 𝑐 2 ] 𝑠 − 1] = 0. (30.14) (30.15) (30.16) (30.17) Solving this quadratic equation for 𝑠 provides the intercepts for the nearest point on the ellipsoid and the opposite point of the ellipsoid where the normal vector, 𝐗𝑛, also points toward. Currently, this method has been implemented for the case of an infinite plane, a cylinder, a sphere, and an ellipsoid with appropriate simplifications. The ellipsoid is intended to be used with rigid body dummy models. The methods are, however, quite general so that many more shapes could be implemented. A direct coupling to solids modeling packages should also be possible in the future. LS-DYNA Theory Manual Nodal Constraints 31 Nodal Constraints In this section nodal constraints and linear constraint equations are described. 31.1 Nodal Constraint Sets This option forces groups of nodes to move together with a common translational acceleration in either one or more degrees of freedom. The implementa- tion is straightforward with the common acceleration defined by 𝑎𝑖common = 𝑎𝑖 ∑ 𝑀𝑗 ∑ 𝑀𝑗 , (31.1) where 𝑛 is the number of nodes, 𝑎𝑖 ith direction, and 𝑎𝑖common is the common acceleration. 𝑗 is the acceleration of the jth constrained node in the Nodal constraint sets eliminate rigid body rotations in the body that contains the node set and, therefore, must be applied very cautiously. 31.2 Linear Constraint Equations Linear constraint equations of the form: ∑ 𝐶𝑘 𝑘=1 𝑢𝑘 = 𝐶0, (31.2) can be defined where 𝑛 is the number of constrained degrees of freedom, 𝑢𝑘 is a constrained nodal displacement, and the 𝐶𝑘 are user-defined coefficients. Unless LS- Nodal Constraints LS-DYNA Theory Manual DYNA is initialized by linking to an implicit code to satisfy this equation at the beginning of the calculation, the constant 𝐶0 is assumed to be zero. The first constrained degree of freedom is eliminated from the equations of motion: 𝑢1 = 𝐶0 − ∑ 𝑘=2 𝐶𝑘 𝐶1 𝑢𝑘. Its velocities and accelerations are given by 𝑢̇1 = − ∑ 𝑘=2 𝑢̈1 = − ∑ 𝑘=2 𝐶𝑘 𝐶1 𝐶𝑘 𝐶1 𝑢̇𝑘, 𝑢̈𝑘 (31.3) (31.4) respectively. In the implementation a transformation matrix 𝐋 is constructed relating the unconstrained 𝑢 and constrained 𝑢constrained degrees of freedom. The constrained accelerations used in the above equation are given by: 𝑢constrained = [𝐋T𝐌𝐋] −1 𝐋T𝐅, (31.5) where 𝐌 is the diagonal lumped mass matrix and 𝐅 is the righthand side force vector. This requires the inversion of the condensed mass matrix which is equal in size to the number of constrained degrees of freedom minus one. The inverse of the condensed mass matrix is computed in the initialization phase and stored in core. LS-DYNA Theory Manual Vectorization and Parallelization 32 Vectorization and Parallelization 32.1 Vectorization In 1978, when the author first vectorized DYNA3D on the CRAY-1, a four-fold increase in speed was attained. This increase was realized by recoding the solution phase to process vectors in place of scalars. It was necessary to process elements in groups rather than individually as had been done earlier on the CDC-7600 supercomputers. Since vector registers are generally some multiple of 64 words, vector lengths of 64 or some multiple are appropriate. In LS-DYNA, groups of 128 elements or possibly some larger integer multiple of 64 are utilized. Larger groups give a marginally faster code, but can reduce computer time sharing efficiency because of increased core requirements. If elements within the group reference more than one material model, subgroups are formed for consecutive elements that reference the same model. LS- DYNA internally sorts elements by material to maximize vector lengths. Conceptually, vectorization is straightforward. Each scalar operation that is normally executed once for one element, is repeated for each element in the group. This means that each scalar is replaced by an array, and the operation is put into a DO-loop. For example, the nodal force calculation for the hexahedron element appeared in a scalar version of DYNA3D as: E11=SGV1*PX1+SGV4*PY1+SGV6*PZ1 E21=SGV2*PY1+SGV4*PX1+SGV5*PZ1 E31=SGV3*PZ1+SGV6*PX1+SGV5*PY1 E12=SGV1*PX2+SGV4*PY2+SGV6*PZ2 E22=SGV2*PY2+SGV4*PX2+SGV5*PZ2 E32=SGV3*PZ2+SGV6*PX2+SGV5*PY2 E13=SGV1*PX3+SGV4*PY3+SGV6*PZ3 E23=SGV2*PY3+SGV4*PX3+SGV5*PZ3 E33=SGV3*PZ3+SGV6*PX3+SGV5*PY3 Vectorization and Parallelization LS-DYNA Theory Manual E14=SGV1*PX4+SGV4*PY4+SGV6*PZ4 E24=SGV2*PY4+SGV4*PX4+SGV5*PZ4 E34=SGV3*PZ4+SGV6*PX4+SGV5*PY4 and in the vectorized version as: DO 110 I = LFT, LLT E11(I)=SGV1(I)*PX1(I)+SGV4(I)*PY1(I)+SGV6(I)*PZ1(I) E21(I)=SGV2(I)*PY1(I)+SGV4(I)*PX1(I)+SGV5(I)*PZ1(I) E31(I)=SGV3(I)*PZ1(I)+SGV6(I)*PX1(I)+SGV5(I)*PY1(I) E12(I)=SGV1(I)*PX2(I)+SGV4(I)*PY2(I)+SGV6(I)*PZ2(I) E22(I)=SGV2(I)*PY2(I)+SGV4(I)*PX2(I)+SGV5(I)*PZ2(I) E32(I)=SGV3(I)*PZ2(I)+SGV6(I)*PX2(I)+SGV5(I)*PY2(I) E13(I)=SGV1(I)*PX3(I)+SGV4(I)*PY3(I)+SGV6(I)*PZ3(I) E23(I)=SGV2(I)*PY3(I)+SGV4(I)*PX3(I)+SGV5(I)*PZ3(I) E33(I)=SGV3(I)*PZ3(I)+SGV6(I)*PX3(I)+SGV5(I)*PY3(I) E14(I)=SGV1(I)*PX4(I)+SGV4(I)*PY4(I)+SGV6(I)*PZ4(I) E24(I)=SGV2(I)*PY4(I)+SGV4(I)*PX4(I)+SGV5(I)*PZ4(I) E34(I)=SGV3(I)*PZ4(I)+SGV6(I)*PX4(I)+SGV5(I)*PY4(I) 110 where 1 ≤ LFT ≤ LLT ≤ n. Elements LFT to LLT inclusive use the same material model and n is an integer multiple of 64. Gather operations are vectorized on most supercomputers. In the gather operation, variables needed for processing the element group are pulled from global arrays into local vectors. For example, the gather operation: DO 10 I X1(I) = Y1(I) = = Z1(I) VX1(I) = VY1(I) = VZ1(I) = = X2(I) = Y2(I) = Z2(I) VX2(I) = VY2(I) = VZ2(I) = = X3(I) = X3(I) = X3(I) = X8(I) = Y8(I) Z8(I) = VX8(I) = LFT, LLT = X(1,IX1(I)) X(2,IX1(I)) X(3,IX1(I)) V(1,IX1(I)) V(2,IX1(I)) V(3,IX1(I)) X(1,IX2(I)) X(2,IX2(I)) X(3,IX2(I)) V(1,IX2(I)) V(2,IX2(I)) V(3,IX2(I)) X(1,IX3(I)) X(2,IX3(I)) X(3,IX3(I)) X(1,IX8(I)) X(2,IX8(I)) X(3,IX8(I)) V(1,IX8(I)) LS-DYNA Theory Manual Vectorization and Parallelization VY8(I) = VZ8(I) = V(2,IX8(I)) V(3,IX8(I)) 10 initializes the nodal velocity and coordinate vector for each element in the subgroup LFT to LLT. In the scatter operation, element nodal forces are added to the global force vector. The force assembly does not vectorize unless special care is taken as described below. In general, the element force assembly is given in FORTRAN by: DO 30 I = 1,NODFRC DO 20 N = 1,NUMNOD DO 10 L = LFT,LLT RHS(I,IX(N,L))=RHS(I,IX(N,L))+FORCE(I,N,L) CONTINUE CONTINUE CONTINUE 10 20 30 where NODFRC is the number of force components per node (3 for solid elements, 6 for shells), LFT and LLT span the number of elements in the vector block, NUMNOD is the number of nodes defining the element, FORCE contains the force components of the individual elements, and RHS is the global force vector. This loop does not vectorize since the possibility exists that more that one element may contribute force to the same node. FORTRAN vector compilers recognize this and will vectorize only if directives are added to the source code. If all elements in the loop bounded by the limits LFT and LLT are disjoint, the compiler directives can be safely added. We therefore attempt to sort the elements as shown in Figure 32.1 to guarantee disjointness. ELEMENT BLOCKING FOR VECTORIZATION Vectorization and Parallelization LS-DYNA Theory Manual Block 1 Block 2 Block 3 Block 3 Figure 32.1. Group of 48 elements broken into 4 disjoint blocks. The current implementation was strongly motivated by Benson [1989] and by work performed at General Motors [Ginsberg and Johnson 1988, Ginsberg and Katnik 1989], where it was shown that substantial improvements in execution speed could be realized by blocking the elements in the force assembly. Katnik implemented element sorting in a public domain version of DYNA3D for the Belytschko-Tsay shell element and added compiler directives to force vectorization of the scatter operations associated with the addition of element forces into the global force vector. The sorting was performed immediately after the elements were read in so that subsequent references to the stored element data were sequential. Benson performed the sorting in the element loops via indirect addressing. In LS-DYNA the published GM approach is taken. Implementation of the vectorization of the scatter operations is implemented in for all elements including the solid, shell, membrane, beam, and truss elements. The sorting is completely transparent to the user. 32.2 Parallelization In parallelization, the biggest hurdle is overcoming Amdahl’s law for multitasking [Cray Research Inc. 1990] 𝑆𝑚 = 𝑓𝑠 + , 𝑓𝑝 (32.1) where LS-DYNA Theory Manual Vectorization and Parallelization 𝑆𝑚 = maximum expected speedup from multitasking 𝑁 = number of processors available for parallel execution 𝑓𝑝 = fraction of a program that can execute in parallel 𝑓𝑠 = fraction of a program that is serial Table 29.1 shows that to obtain a speed factor of four on eight processors it is necessary to have eighty-six percent of the job running in parallel. Obviously, to gain the highest speed factors the entire code must run in parallel. LS-DYNA has been substantially written to function on all shared memory parallel machine architectures. Generally, shared memory parallel speed-ups of 5 on 8 processors are possible but this is affected by the machine characteristics. We have observed speeds of 5.6 on full car crash models on a machine of one manufacturer only to see a speed-up of 3.5 on a different machine of another manufacturer. % N = 2 N = 4 N = 8 N = 16 N = 32 N = 64 N = 12 N = 256 1.75 86.0% 1.82 90.0% 1.85 92.0% 1.89 94.0% 1.92 96.0% 1.96 98.0% 1.98 99.0% 1.98 99.2% 1.99 99.4% 1.99 99.6% 1.99 99.7% 2.00 99.8% 99.9% 2.00 100.0% 2.00 2.82 3.08 3.23 3.39 3.57 3.77 3.88 3.91 39.3 3.95 3.96 3.98 3.99 4.00 4.04 4.71 5.13 5.63 6.25 7.02 7.48 7.58 7.68 7.78 7.84 7.89 7.94 8.00 5.16 6.40 7.27 8.42 10.00 12.31 13.91 14.29 14.68 15.09 15.31 15.53 15.76 16.00 5.99 7.80 9.20 11.19 14.29 19.75 24.43 25.64 26.98 28.47 29.28 30.13 31.04 32.00 6.52 8.77 10.60 13.39 18.18 28.32 39.26 42.55 46.44 51.12 53.83 56.84 60.21 64.00 8 6.82 9.34 11.47 14.85 21.05 36.16 56.39 63.49 72.64 84.88 92.69 102.07 113.58 128.00 6.98 9.66 11.96 15.71 22.86 41.97 72.11 84.21 101.19 126.73 145.04 169.54 203.98 256.00 Table 29.1.Maximum theoretical speedup Sm, on N CPUs with parallelism [Cray Research Inc. 1990]. In the element loops element blocks with vector lengths of 64 or some multiple are assembled and sent to separate processors. All elements are processed in parallel. On the average a speed factor of 7.8 has been attained in each element class corresponding to 99.7% parallelization. A significant complication in parallelizing code is that a variable can sometimes be updated simultaneously by different processors with incorrect results. To force the processors to access and update the variable in a sequential manner, a GUARD compiler directive must be introduced. This results in an interruption to the parallel Vectorization and Parallelization LS-DYNA Theory Manual execution and can create a bottleneck. By sorting the data in the parallel groups or by allocating additional storage it is usually possible to eradicate the GUARDS from the coding. The effort may not be worth the gains in execution speed. The element blocks are defined at the highest level and each processor updates the entire block including the right hand side force assembly. The user currently has two options: GUARD compiler directives prevent simultaneous updates of the RHS vector (recommended for single CPU processors or when running in a single CPU mode on a multi-processor), or assemble the right hand side in parallel and let LS- DYNA prevent conflicts between CPU’s. This usually provides the highest speed and is recommended, i.e., no GUARDS. When executing LS-DYNA in parallel, the order of operations will vary from run to run. This variation will lead to slightly different numerical results due to round-off errors. By the time the calculation reaches completion variations in nodal accelerations and sometimes even velocities are observable. These variations are independent of the precision and show up on both 32 and 64 bit machines. There is an option in LS-DYNA to use an ordered summation of the global right hand side force vector to eliminate numerical differences. To achieve this the element force vectors are stored. After leaving the element loop, the global force vector is assembled in the same order that occurs on one processor. The ordered summation option is slower and uses more memory than the default, but it leads to nearly identical, if not identical, results run to run. Parallelization in LS-DYNA was initially done with vector machines as the target where the vector speed up is typically 10 times faster than scalar. On vector machines, therefore, vectorization comes first. If the problem is large enough then parallelization is automatic. If vector lengths are 128, for example, and if 256 beam elements are used only a factor of 2 in speed can be anticipated while processing beam elements. Large contact surfaces will effectively run in parallel, small surfaces having under 100 segments will not. The speed up in the contact subroutines has only registered 7 on 8 processors due to the presence of GUARD statements around the force assembly. Because real models often use many special options that will not even vectorize efficiently it is unlikely that more than 95% of a given problem will run in parallel on a shared memory parallel machine. LS-DYNA Theory Manual Airbags 33 Airbags Additional information on the airbag modeling and comparisons with experimental data can be found in a report [Hallquist, Stillman, Hughes, and Tarver 1990] based on research sponsored by the Motor Vehicles Manufacturers Association (MVMA). 33.1 Control Volume Modeling A direct approach for modeling the contents of the airbag would be to discretize the interior of the airbag using solid elements. The total volume and pressure-volume relationship of the airbag would then be the sum of all the elemental contributions. Although this direct approach could be applied in a straight forward manner to an inflated airbag, it would become very difficult to implement during the inflation phase of the airbag deployment. Additionally, as the model is refined, the solid elements would quickly overwhelm all other computational costs and make the numerical simulations prohibitively expensive. An alternative approach for calculating the airbag volume, that is both applicable during the inflation phase and less computationally demanding, treats the airbag as a control volume. The control volume is defined as the volume enclosed by a surface. In the present case, the ‘control surface’ that defines the control volume is the surface modeled by shell or membrane elements comprising the airbag fabric material. Because the evolution of the control surface is known, i.e., the position, orientation, and current surface area of the airbag fabric elements are computed and stored at each time step, we can take advantage of these properties of the control surface elements to calculate the control volume, i.e., the airbag volume. The area of the control surface can be related to the control volume through Green’s Theorem ∭ 𝜙 ∂𝜓 ∂𝑥 𝑑𝑥𝑑𝑦𝑑𝑧 = − ∭ 𝜓 ∂𝜙 ∂𝑥 𝑑𝑥𝑑𝑦𝑑𝑧 + ∮ 𝜙𝜓𝑛𝑥𝑑𝛤 , (33.1) Airbags LS-DYNA Theory Manual where the first two integrals are integrals over a closed volume, i.e., 𝑑𝑣 = 𝑑𝑥𝑑𝑦𝑑𝑧, the last integral is an integral over the surface enclosing the volume, and 𝑛𝑥 is the direction cosine between the surface normal and the 𝑥 direction (corresponding to the x-partial derivative); similar forms can be written for the other two directions. The two arbitrary functions 𝜙 and 𝜓 need only be integrated over the volume and surface. The integral form of the volume can be written as 𝑉 = ∭ 𝑑𝑥𝑑𝑦𝑑𝑧. (33.2) Comparing the first of the volume integrals in Equation (33.1) to Equation (33.2), we can easily obtain the volume integral from Equation (33.1) by choosing for the two arbitrary functions 𝜙 = 1, 𝜓 = 𝑥𝑥, leading to 𝑉 = ∫ ∫ ∫ 𝑑𝑥𝑑𝑦𝑑𝑧 = ∮ 𝑥𝑛𝑥𝑑𝛤 . (33.3) (33.4) (33.5) The surface integral in Equation (33.5) can be approximated by a summation over all the elements comprising the airbag, i.e., ∮ 𝑥𝑛𝑥𝑑𝛤 ≈ ∑ 𝑥̅𝑖𝑛𝑖𝑥𝐴𝑖 , (33.6) 𝑖=1 where for each element i: 𝑥̅𝑖 is the average x coordinate, 𝑛𝑖𝑥 is the direction cosine between the elements normal and the 𝑥 direction, and 𝐴𝑖 is the surface area of the element. Although Equation (33.5) will provide the exact analytical volume for an arbitrary direction, i.e., any 𝑛, the numerical implementation of Equation (33.5), and its approximation Equation (33.6), has been found to produce slightly different volumes, differing by a few percent, depending on the choice of directions: if the integration direction is nearly parallel to a surface element, i.e., the direction cosine is nearly zero, numerical precision errors affect the volume calculation. The implementation uses as an integration direction, a direction that is parallel to the maximum principle moment of inertia of the surface. Numerical experiments have shown this choice of integration direction produces more accurate volumes than the coordinate or other principle inertia directions. Because airbag models may contain holes, e.g., holes for inflation and deflation, and Green’s Theorem only applies to closed surfaces, a special treatment is needed for calculating the volume of airbags with holes. This special treatment consists of the following: LS-DYNA Theory Manual Airbags • The n-sized polygon defining the hole is identified automatically, using edge locating algorithms in LS-DYNA. • The n-sized polygon is projected onto a plane, i.e., it is assumed to be flat; this is a good approximation for typical airbag hole geometries. Planar symmetry should work with the control volume capability for one symmetry plane. • The area of the flat n-sided polygon is calculated using Green’s Theorem in two dimensions. • The resulting holes are processed as another surface element in the airbag control volume calculation. 33.2 Equation of State Model As explained above, at each time step in the calculation the current volume of the airbag is determined from the control volume calculation. The pressure in the airbag corresponding to the control volume is determined from an equation of state (EOS) that relates the pressure to the current gas density (volume) and the specific internal energy of the gas. The equation of state used for the airbag simulations is the usual ‘Gamma Law Gas Equation of State’, 𝑝 = (𝑘 − 1)𝜌𝑒, (33.7) where 𝑝 is the pressure, 𝑘 is a constant defined below, 𝜌 is the density, and 𝑒 is the specific internal energy of the gas. The derivation of this equation of state is obtained from thermodynamic considerations of the adiabatic expansion of an ideal gas. The incremental change in internal energy, 𝑑𝑈, in 𝑛 moles of an ideal gas due to an incremental increase in temperature, 𝑑𝑇, at constant volume is given by where 𝑐v is the specific heat at constant volume. Using the ideal gas law we can relate the change in temperature to a change in the pressure and total volume, 𝑣, as 𝑑𝑈 = 𝑛𝑐v𝑑𝑇, (33.8) 𝑑(𝑝𝑣) = 𝑛𝑅𝑑𝑇, (33.9) where 𝑅 is the universal gas constant. Solving the above for 𝑑𝑇 and substituting the result into Equation (33.8) gives 𝑑𝑈 = 𝑐v𝑑(𝑝𝑣) = 𝑑(𝑝𝑣) (𝑘 − 1) , where we have used the relationship 𝑅 = 𝑐p − 𝑐v, and the notation LS-DYNA Draft (33.10) Airbags LS-DYNA Theory Manual Equation (33.10) may be rewritten as 𝑘 = 𝑐p 𝑐v . and integrated to yield Solving for the pressure 𝑑𝑈 = 𝜌0𝑣0 𝑘 − 1 𝑑 ( ), 𝑒 = 𝜌0𝑣0 = . 𝜌(𝑘 − 1) 𝑝 = (𝑘 − 1)𝜌𝑒. (33.12) (33.13) (33.14) (33.15) The equation of state and the control volume calculation can only be used to determine the pressure when the specific internal energy is also known. The evolution equation for the internal energy is obtained by assuming the change in internal energy is given by 𝑑𝑈 = −𝑝𝑑𝑣, (33.16) where the minus sign is introduced to emphasize that the volume increment is negative when the gas is being compressed. This expression can be written in terms of the specific internal energy as 𝑑𝑒 = 𝑑𝑈 𝜌0𝑣0 = − 𝑝𝑑𝑣 𝜌0𝑣 . Next, we divide the above by the equation of state, Equation (4.11.144), to obtain 𝑑𝑒 = − 𝜌(𝑘 − 1)𝑑𝑣 𝜌0𝑣0 = − (𝑘 − 1)𝑑𝑣 , which may be integrated to yield ln𝑒 = (1 − 𝑘)ln𝑉, or evaluating at two states and exponentiating both sides yields 𝑒2 = 𝑒1 ( (1−𝑘) ) . 𝑣2 𝑣1 (33.17) (33.18) (33.19) (33.20) The specific internal energy evolution equation, Equation (33.20), the equation of state, Equation (4.11.144), and the control volume calculation completely define the pressure-volume relation for an inflated airbag. LS-DYNA Theory Manual Airbags 33.3 Airbag Inflation Model Airbag inflation models have been used for many years in occupant simulation codes such as CAL3D [Fleck, 1981]. The inflation model we chose to implement in LS-DYNA is due to Wang and Nefske[1988] and more recent improvements to the model in LS-DYNA were suggested by Wang [1992]. In their development they consider the mass flow due to the vents and leakage through the bag. We assume that the mass flow rate and the temperature of the gas going into the bag from an inflator are provided as tabulated functions of time. A pressure relation is defined: 𝑄 = 𝑝e 𝑝2 , (33.21) where 𝑝e is the external pressure and 𝑝2 is the internal pressure in the bag. A critical pressure relationship is defined as: 𝑄crit = ( ⁄ ) 𝑘−1 , 𝑘 + 1 where 𝑘 is the ratio of specific heats: 𝑘 = 𝑐p 𝑐v . If 𝑄 ≤ 𝑄crit then 𝑄 = 𝑄crit. Wang and Nefske define the mass flow through the vents and leakage by 𝑚̇ 23 = 𝐶23𝐴23 𝑝2 𝑅√𝑇2 and 𝑘⁄ √2𝑔𝑐 ( 𝑘𝑅 𝑘 − 1 ) (1 − 𝑄 𝑘−1 ⁄ ), 𝑚̇ 23 ′ = 𝐶′23𝐴′23 𝑝2 𝑅√𝑇2 𝑘⁄ √2𝑔𝑐 ( 𝑘𝑅 𝑘 − 1 ) (1 − 𝑄 𝑘−1 ⁄ ), (33.22) (33.23) (33.24) (33.25) where 𝐶23, 𝐴23, 𝐶′23, 𝐴′23, 𝑅 and 𝑔𝑐 are the vent orifice coefficient, vent orifice area, the orifice coefficient for leakage, the area for leakage, the gas constant, and the gravitational conversion constant, respectively. The internal temperature of the airbag gas is denoted by 𝑇2. We note that both 𝐴23 and 𝐴′23 can be defined as a function of pressure [Wang, 1992] or if they are input as zero they are computed within LS-DYNA. This latter option requires detailed modeling of the airbag with all holes included. A uniform temperature and pressure is assumed; therefore, in terms of the total airbag volume 𝑉2 and air mass, 𝑚2, the perfect gas law is applied: Airbags LS-DYNA Theory Manual Solving for 𝑇2: 𝑝2𝑉 = 𝑚2𝑅𝑇2. (33.26) 𝑝2𝑉 𝑚2𝑅 and substituting Equation (33.27) into equations (33.25), we arrive at the mass transient equation: 𝑇2 = (33.27) , 𝑚̇ out = 𝑚̇ 23 + 𝑚̇ 23 ′ = 𝜇√2𝑝2𝜌 √ √ √ ⎷ 𝑘 − 𝑄 𝑘+1 ⁄ ) 𝑘 (𝑄 𝑘 − 1 (33.28) where 𝜌 = density of airbag gas, 𝜇 = bag characterization parameter, 𝑚̇ out = total mass flow rate out of bag. In terms of the constants used by Wang and Nefske: 𝜇 = √𝑔𝑐(𝐶23𝐴23 + 𝐶′23𝐴′23). (33.29) We solved these equations iteratively, via function evaluation. Convergence usually occurs in 2 to 3 iterations. The mass flow rate and gas temperature are defined in load curves as a function of time. Using the mass flow rate we can easily compute the increase in internal energy: 𝐸̇in = 𝑐p𝑚̇ in𝑇in, (33.30) where 𝑇in is the temperature of the gas flowing into the airbag. Initializing the variables pressure, 𝑝, density, 𝜌, and energy, 𝐸, to their values at time 𝑛, we can begin the iterations loop to compute the new pressure, 𝑝𝑛 + 1, at time 𝑛 + 1. 𝑝𝑛+1 2⁄ = 𝜌𝑛+1 2⁄ = 𝐸𝑛+1 2⁄ = 𝑝𝑛 + 𝑝𝑛+1 𝜌𝑛 + 𝜌𝑛+1 𝐸𝑛 + 𝐸𝑛+1 𝑄𝑛+1 2⁄ = max ⎜⎜⎜⎜⎛ 𝑝𝑒 𝑛+1 𝑝2 ⎝ , 𝑄crit . ⎟⎟⎟⎟⎞ ⎠ (33.31) The mass flow rate out of the bag, 𝑚̇ out can now be computed: 𝑛+1 𝑚̇ out 2⁄ 33-6 (Airbags) = 𝜇√2𝑝2 𝑛+1 2⁄ √ √ √ √ ⎷ 𝜌𝑛+1 2⁄ ⎜⎛𝑄𝑛+1 2⁄ ⎝ 𝑘⁄ − 𝑄𝑛+1 2⁄ 𝑘+1 ⁄ 𝑘 − 1 ⎟⎞ ⎠ , LS-DYNA Theory Manual Airbags where and the total mass updated: 𝑛+1 𝑝2 2⁄ = 𝑝𝑛+1 2⁄ + 𝑝e, 𝑛+1 2⁄ 𝑚𝑛+1 = 𝑚𝑛 + Δ𝑡 (𝑚̇ in 𝑚𝑛 + 𝑚𝑛+1 𝑚𝑛+1 2⁄ = . 𝑛+1 − 𝑚out 2⁄ ) The energy exiting the airbag is given by: 2⁄ 𝐸𝑛+1 2⁄ 𝑚𝑛+1 2⁄ we can now compute our new energy at time 𝑛 + 1 𝑛+1 = 𝑚̇ out 𝑛+1 out 2⁄ 𝐸̇ , 𝐸𝑛+1 = 𝐸𝑛 + Δ𝑡 (Ė 2⁄ n+1 in − 𝐸̇ 2⁄ 𝑛+1 out ) − 𝑝𝑛+1 2⁄ Δ𝑉𝑛+1 2⁄ , (33.33) (33.34) (33.35) (33.36) where Δ𝑉𝑛+1 be computed: 2⁄ is the change in volume from time 𝑛 to 𝑛 + 1. The new pressure can now 𝑝𝑛+1 = (𝑘 − 1) 𝐸𝑛+1 𝑉𝑛+1, (33.37) which is the gamma-law (where 𝑘 = 𝛾) gas equation. This ends the iteration loop. 33.4 Wang's Hybrid Inflation Model Wang's proposed hybrid inflator model [1995a, 1995b] provides the basis for the model in LS-DYNA. The first law of thermodynamics is used for an energy balance on the airbag control volume. 𝑑𝑡 where (𝑚𝑢)cv = ∑ 𝑚̇ 𝑖 ℎ𝑖 − ∑ 𝑚̇ 𝑜 ℎ𝑜 − 𝑊̇ cv − 𝑄̇cv, (33.38) 𝑑𝑡 (𝑚𝑢)cv = rate of change of airbag internal energy ∑ 𝑚𝑖 ℎ𝑖 = energy into airbag by mass flow (e. g. , inflator) ∑ 𝑚𝑜 ℎ𝑜 = energy out of airbag by mass flow (e. g. , vents) 𝑊̇ cv = ∫ 𝑃𝑑𝑉̇ = work done by airbag expansion 𝑄̇cv = energy out by heat transfer through airbag surface. Airbags LS-DYNA Theory Manual The rate of change of internal energy, the left hand side of Equation (33.38), can be differentiated: 𝑑𝑡 𝑑𝑚 𝑑𝑡 where we have used the definition (𝑚𝑢) = 𝑑𝑚 𝑑𝑡 𝑢 + 𝑚 𝑑𝑢 𝑑𝑡 = 𝑢 + 𝑚 𝑑𝑡 (𝑐v𝑇) = 𝑚̇𝑢 + 𝑚𝑐 ̇v𝑇 + 𝑚𝑐v 𝑑𝑇 𝑑𝑡 , 𝑢 = 𝑐v𝑇. (33.39) (33.40) Then, the energy equation can be re-written for the rate of change in temperature for the airbag = 𝑑𝑇cv 𝑑𝑡 ∑ 𝑚̇ 𝑖 ℎ𝑖 − ∑ 𝑚̇ 𝑜 ℎ𝑜 − 𝑊̇ cv − 𝑄̇cv − (𝑚̇𝑢)cv − (𝑚𝑐 ̇v𝑇)cv (𝑚𝑐v)cv Temperature dependent heat capacities are used. The constant pressure molar heat capacity is taken as: (33.41) 𝑐 ̅p = 𝑎 ̅ + 𝑏̅𝑇, and the constant volume molar heat capacity as: 𝑐 ̅v = 𝑎 ̅ + 𝑏̅𝑇 − 𝑟 ̅, where 𝑟 ̅ = gas constant = 8.314 J/gm-mole K 𝑎 ̅ = constant [J/gm-mole K] 𝑏̅ = constant [J/gm-mole K2] (33.42) (33.43) Mass based values are obtained by dividing the molar quantities by the molecular weight, 𝑀, of the gas 𝑎 = 𝑎 ̅ , 𝑏 = 𝑏̅ , 𝑟 = 𝑟 ̅ . The constant pressure and volume specific heats are then given by 𝑐p = 𝑎 + 𝑏𝑇 𝑐v = 𝑎 + 𝑏𝑇 − 𝑟. The specific enthalpy and internal energy becomes: ℎ = ∫ 𝑐𝑝𝑑𝑇 = 𝑎𝑇 + 𝑏𝑇2 𝑢 = ∫ 𝑐𝑣𝑑𝑇 = 𝑎𝑇 + 𝑏𝑇2 − 𝑟𝑇. (33.44) (33.45) (33.46) (33.47) (33.48) For ideal gas mixtures the molecular weight is given as: LS-DYNA Theory Manual Airbags 𝑀 = , ∑ 𝑓𝑖 𝑀𝑖 and the constant pressure and volume specific heats as: 𝑐p = ∑ 𝑓𝑖 𝑐p(𝑖) 𝑐v = ∑ 𝑓𝑖 𝑐v(𝑖), where 𝑓𝑖 = mass fraction of gas 𝑖 𝑀𝑖 = molecular weight of gas 𝑖 𝑐p(𝑖) = constant pressure specific heat of gas 𝑖 𝑐v(𝑖) = constant volume specific heat of gas 𝑖. (33.49) (33.50) (33.51) The specific enthalpy and internal energy for an ideal gas mixture with temperature dependent heat capacity are ℎ = ∫ ∑ 𝑓𝑖 𝑐p(𝑖)𝑑𝑇 = ∑ 𝑓𝑖 (𝑎𝑖𝑇 + 𝑏𝑖𝑇2 ) 𝑢 = ∫ ∑ 𝑓𝑖 𝑐v(𝑖)𝑑𝑇 = ∑ 𝑓𝑖 (𝑎𝑖𝑇 + 𝑏𝑖𝑇2 − 𝑟𝑖𝑇). The rate of change of temperature for the airbag is 𝑑𝑇cv 𝑑𝑡 = ∑ 𝑚̇ 𝑖 ℎ𝑖 − ∑ 𝑚̇ 𝑜 ℎ𝑜 − 𝑊̇ cv − 𝑄̇cv − (𝑚̇𝑢)cv − (𝑚𝑐 ̇v𝑇)cv (𝑚𝑐v)cv . The energy in by mass flow becomes: ∑ 𝑚̇ 𝑖 ℎ𝑖 = ∑ 𝑚̇ 𝑖 (𝑎𝑖𝑇𝑖 + 𝑏𝑖𝑇𝑖 ), 𝑚̇ 𝑖 is specified by an inflator mass inflow vs. time table 𝑇𝑖 is specified by an inflator temperature vs. time table 𝑎, 𝑏 are input constants for gas 𝑖 And the energy out by mass flow: ∑ 𝑚̇ 𝑜 ℎ𝑜 = ∑ 𝑚̇ 𝑜 [ ∑ 𝑓𝑖 (𝑎𝑖𝑇𝑐𝑣 + gases 𝑏𝑖𝑇cv ) ]. (33.52) (33.53) (33.54) (33.55) (33.56) The gas leaves the airbag at the control volume temperature 𝑇𝑐𝑣. The mass flow rate out through vents and fabric leakage is calculated by the one dimensional Airbags LS-DYNA Theory Manual isentropic flow equations per Wang and Nefske. The work done by the airbag expansion is given by: 𝑊̇ cv = ∫ 𝑃𝑑𝑉̇ , (33.57) 𝑃 is calculated by the equation of state for a perfect gas, 𝑝 = 𝜌𝑅𝑇 and 𝑉̇ is calculated by LS-DYNA For the energy balance, we must compute the energy terms (𝑚̇ 𝑢)cv and (𝑚𝑐v)cv. Conservation of mass leads to: 𝑚̇ cv = 𝑚̇ 𝑖 − 𝑚̇ 𝑜 𝑚cv = ∫ 𝑚̇ cv 𝑑𝑡. The internal energy is given by 𝑢cv = ∑ 𝑓𝑖 (𝑎𝑖𝑇cv + 𝑏𝑖𝑇cv − 𝑟𝑖𝑇cv), and the heat capacity at contact volume is: (𝑐v)cv = ∑ 𝑓𝑖 (𝑎𝑖 + 𝑏𝑖𝑇cv − 𝑟𝑖). (33.58) (33.59) (33.60) 33.5 Constant Volume Tank Test Constant volume tank tests are used to characterize inflators. The inflator is ignited within the tank and, as the propellant burns, gas is generated. The inflator temperature is assumed to be constant. From experimental measurements of the time history of the tank pressure it is straightforward to derive the mass flow rate, 𝑚̇ . From energy conservation, where 𝑇i and 𝑇t are defined to be the temperature of the inflator and tank, respectively, we obtain: 𝑐p𝑚̇𝑇i = 𝑐v𝑚̇𝑇t + 𝑐v𝑚𝑇̇t. For a perfect gas under constant volume, 𝑉̇ = 0, hence, 𝑝̇𝑉 = 𝑚̇𝑅𝑇t + 𝑚𝑅𝑇̇t, and, finally, we obtain the desired mass flow rate: 𝑚̇ = 𝑐v𝑝̇𝑉 𝑐p𝑅𝑇i . (33.61) (33.62) (33.63) LS-DYNA Theory Manual Dynamic Relaxation and System Damping 34 Dynamic Relaxation and System Damping Dynamic relaxation allows LS-DYNA to approximate solutions to linear and nonlinear static or quasi-static processes. Control parameters must be selected with extreme care or bad results can be obtained. The current methods are not compatible with displacement or velocity boundary conditions, but various body loads, thermal loads, pressures, and nodal loads are allowed. The solutions to most nonlinear problems are path dependent, thus results obtained in the presence of dynamic oscillations may not be the same as for a nonlinear implicit code, and they may diverge from reality. In LS-DYNA we have two methods of damping the solution. The first named “dynamic relaxation” is used in the beginning of the solution phase to obtain the initial stress and displacement field prior to beginning the analysis. The second is system damping which can be applied anytime during the solution phase either globally or on a material basis. 34.1 Dynamic Relaxation For Initialization In this phase only a subset of the load curves is used to apply the static load which is flagged in the load curve section of the manual. The calculation begins and executes like a normal LS-DYNA calculation but with damping incorporated in the update of the displacement field. Our development follows the work of Underwood [1986] and Papadrakakis [1981] with the starting point being the dynamic equilibrium equation, Equation (23.1) with the addition of a damping term, at time 𝑛: 𝐌𝐚𝑛 + 𝐂𝐯𝑛 + 𝐐𝑛(𝐝) = 0, (34.1) Dynamic Relaxation and System Damping LS-DYNA Theory Manual 𝐐𝑛(𝐝) = 𝐅𝑛 − 𝐏𝑛 − 𝐇𝑛, (34.2) where we recall that 𝐌 is the mass matrix, 𝐂 is the damping matrix, 𝑛 indicates the nth time step, 𝐚𝑛 is the acceleration, 𝐯𝑛 the velocity, and 𝐝 is the displacement vector. With Δ𝑡 as the fixed time increment we get for the central difference scheme: 𝐯𝑛+1 2⁄ = (𝐝𝑛+1 − 𝐝𝑛) Δ𝑡 ; 𝐚𝑛 = For 𝐯𝑛 we can assume an averaged value (𝐯𝑛+1 2⁄ − 𝐯𝑛−1 Δ𝑡 2⁄ ) . and obtain 𝐯𝑛 = (𝐯𝑛+1 2⁄ + 𝐯𝑛−1 2⁄ ), 𝐯𝑛+1 2⁄ = ( Δ𝑡 𝐌 + −1 𝐂) [( Δ𝑡 𝐌 − 𝐂) 𝐯𝑛−1 2⁄ − 𝐐𝑛], 𝐝𝑛+1 = 𝐝𝑛 + Δ𝑡𝐯𝑛+1 2⁄ . (34.3) (34.4) (34.5) (34.6) In order to preserve the explicit form of the central difference integrator, 𝐌 and 𝐂 must be diagonal. For the dynamic relaxation scheme 𝐂 has the form If Equation (34.7) is substituted into (34.5) the following form is achieved 𝐂 = 𝑐 ⋅ 𝐌. 𝐯𝑛+1 2⁄ = 2 − 𝑐Δ𝑡 2 + 𝑐Δ𝑡 𝐯𝑛−1 2⁄ + 2Δ𝑡 2 + 𝑐Δ𝑡 ⋅ 𝐌−1 ⋅ 𝐐𝑛. (34.7) (34.8) Since 𝐌 is diagonal, each solution vector component may be computed individually from 𝑛+1 𝐯𝑖 2⁄ = 2 − 𝑐Δ𝑡 2 + 𝑐Δ𝑡 𝑛−1 𝐯𝑖 2⁄ + 2Δ𝑡 2 + 𝑐Δ𝑡 𝐐𝑖 𝑚𝑖 . As a starting procedure it is suggested by Underwood 𝐯0 = 0 𝐝0 = 0. (34.9) (34.10) Since the average value is used for 𝐯𝑛, which must be zero at the beginning for a quasi- static solution thus the velocity at time +1 ⁄ 2 is 𝐯−1 2⁄ = −𝐯 2⁄ , 2⁄ = − Δ𝑡 𝐌−1𝐐𝑜. (34.11) (34.12) A damping coefficient must now be selected to obtain convergence to the static solution in minimal time. The best estimate for damping values is based on the frequencies of LS-DYNA Theory Manual Dynamic Relaxation and System Damping the structure. One choice is to focus on an optimal damping parameter as suggested by Papadrakakis [1981]. Then dynamic relaxation is nothing else but a critically damped dynamic system 𝐶 = 𝐶cr = 2𝜔min𝑚, (34.13) with 𝑚 as modal mass. The problem is finding the dominant eigenvalue in the structure related to the “pseudo-dynamic” behavior of the structure. As the exact estimate would be rather costly and not fit into the explicit algorithm, an estimate must be used. Papadrakakis suggests 𝜆𝐷 = ∥𝐝𝑛+1 − 𝐝𝑛∥ ∥ 𝐝𝑛 − 𝐝𝑛−1∥ . (34.14) When this quantity has converged to an almost constant value, the minimum eigenvalue of the structure can be estimated: 2 = − 𝜔min (𝜆𝐷 2 − 𝜆𝐷 ⋅ 𝛽 + 𝛼) , 𝜆𝐷 ⋅ 𝛾 where 𝛼 = 2 − 𝑐Δ𝑡 2 + 𝑐Δ𝑡 𝛽 = 𝛼 + 1 2Δ𝑡2 2 + 𝑐Δ𝑡 𝛾 = . (34.15) (34.16) The maximum eigenvalue determines the time step and is already known from the model 𝜔max 2 = 4.0 (Δ𝑡)2. Now the automatic adjustment of the damping parameter closely follows the paper of Papadrakakis, checking the current convergence rate compared to the optimal convergence rate. If the ratio is reasonably close, then an update of the iteration parameters is performed. (34.17) . 𝑐 = 4.0 Δ𝑡 √𝜔min (𝜔min ⋅ 𝜔max 2 + 𝜔max ) As is clearly visible from Equation (34.18) the value of highest frequency has always a rather high influence on the damping ratio. This results in a non-optimal damping ratio, if the solution is dominated by the response in a very low frequency compared to the highest frequency of the structure. This is typically the case in shell structures, when bending dominates the solution. It was our observation that the automatic choice following Papadrakakis results in very slow convergence for such structures, and this is also mentioned by Underwood for similar problems. The damping ratio should then be fully adjusted to the lowest frequency by hand by simply choosing a rather high (34.18) Dynamic Relaxation and System Damping LS-DYNA Theory Manual damping ratio. An automatic adjustment for such cases is under preparation. For structures with dominant frequencies rather close to the highest frequency, convergence is really improved with the automatically adjusted parameter. If the automated approach is not used then we apply the damping as 𝐯𝑛+1 2⁄ = 𝜂𝐯𝑛−1 2⁄ + 𝐚𝑛Δ𝑡, (34.19) where 𝜂 is an input damping factor (defaulted to .995). The factor, 𝜂, is equivalent to the corresponding factor in Equations (31.7- 31.8). The relaxation process continues until a convergence criterion based on the global kinetic energy is met, i.e., convergence is assumed if 𝐸ke < CVTOL ⋅ 𝐸𝑘𝑒 max, (34.20) where CVTOL is the convergence tolerance (defaulted to .001). The kinetic energy excludes any rigid body component. Initial velocities assigned in the input are stored during the relaxation. Once convergence is attained the velocity field is initialized to the input values. A termination time for the dynamic relaxation phase may be included in the input and is recommended since if convergence fails, LS-DYNA will continue to execute indefinitely. 34.2 Mass Weighted Damping With mass weighted damping, the Equation (23.2) is modified as: 𝐚𝑛 = 𝐌−1(𝐏𝑛 − 𝐅𝑛 + 𝐇𝑛 − 𝐅damp ), where 𝐹damp = 𝐷𝑠𝑚𝑣. (34.21) (34.22) As seen from Figure 34.1 and as discussed above the best damping constant for the system is usually the critical damping constant: Therefore, 𝐷𝑠 = 2𝜔min (34.23) is recommended. 34.3 Dynamic Relaxation—How Fast Does it Converge? LS-DYNA Theory Manual Dynamic Relaxation and System Damping The number of cycles required to reduce the amplitude of the dynamic response by a factor of 10 can be approximated by [see Stone, Krieg, and Beisinger 1985] ncycle = 1.15 𝜔max 𝜔min . (34.24) Structural problems which involve shell and beam elements can have a very large ratio and consequently very slow convergence. Figure 34.1. Displacement versus time curves with a variety of damping coefficients applied to a one degree-of-freedom oscillator. LS-DYNA Theory Manual Heat Transfer 35 Heat Transfer LS-DYNA can be used to solve for the steady state or transient temperature field on three-dimensional geometries. Material properties may be temperature dependent and either isotropic or orthotropic. A variety of time and temperature dependent boundary conditions can be specified including temperature, flux, convection, and radiation. The implementation of heat conduction into LS-DYNA is based on the work of Shapiro [1985]. 35.1 Conduction of Heat in an Orthotropic Solid The differential equations of conduction of heat in a three-dimensional continuum is given by 𝜌𝑐𝑝 ∂𝜃 ∂𝑡 = (𝑘𝑖𝑗𝜃,𝑗) ,𝑖 + 𝑄 (35.1) subject to the boundary conditions, 𝜃 = 𝜃𝑠 on Γ1, 𝑘𝑖𝑗𝜃,𝑗𝑛𝑖 + 𝛽𝜃 = 𝛾 on Γ2, and initial conditions at 𝑡0: 𝜃Γ = 𝜃0(𝑥𝑖) at 𝑡 = 𝑡0. (35.2) where 𝜃 = 𝜃(𝑥𝑖, 𝑡) temperature 𝑥𝑖 = 𝑥𝑖(𝑡) coordinates as a function of time 𝜌 = 𝜌(𝑥𝑖) density 𝑐𝑝 = 𝑐𝑝(𝑥𝑖, 𝜃) specific heat capacity 𝑘𝑖𝑗 = 𝑘𝑖𝑗(𝑥𝑖, 𝜃) thermal conductivity 𝑄 = 𝑄(𝑥𝑖, 𝜃) internal heat generation rate per unit volume Ω 𝜃Γ = prescribed temperature on Γ1 𝑛𝑖 = normal vector to Γ2 Equations (35.1)-(35.2) represent the strong form of a boundary value problem to be solved for the temperature field within the solid. Heat Transfer LS-DYNA Theory Manual DYNA3D employs essentially the same theory as TOPAZ [Shapiro 1985] in solving Equation (35.1) by the finite element method. Those interested in a more detailed description of the theory are referred to the TOPAZ User’s Manual. Brick elements are integrated with a 2 × 2 × 2 Gauss quadrature rule, with temperature dependence of the properties accounted for at the Gauss points. Time integration is performed using a generalized trapezoidal method shown by Hughes to be unconditionally stable for nonlinear problems. Newton’s method is used to satisfy equilibrium in nonlinear problems. The finite element method provides the following equations for the numerical solution of Equations (35.1)-(35.2) [ 𝐶𝑛+𝛼 Δ𝑡 + 𝛼𝐻𝑛+𝛼] {𝜃𝑛+1 − 𝜃𝑛} = {𝐹𝑛+𝛼 − 𝐻𝑛+𝛼𝜃𝑛} where 𝑒 ] [𝐶] = ∑[𝐶𝑖𝑗 = ∑ ∫ 𝑁𝑖𝜌𝑐𝑁𝑗𝑑Ω Ω𝑒 𝑒 ] [𝐻] = ∑[𝐻𝑖𝑗 = ∑ ⎢⎡ ∫ ∇𝑇𝑁𝑖𝐾∇𝑁𝑗𝑑Ω + ∫ 𝑁𝑖𝛽𝑁𝑗𝑑Γ ⎣ Ω𝑒 Γ𝑒 ⎥⎤ ⎦ 𝑒] [𝐹] = ∑[𝐹𝑖 = ∑ ⎢⎡ ∫ 𝑁𝑖𝑞𝑔𝑑Ω + ∫ 𝑁𝑖𝛾𝑑Γ ⎣ Ω𝑒 Γ𝑒 ⎥⎤ ⎦ (35.3) (35.4) (35.5) (35.6) The parameter 𝛼 is taken to be in the interval [0,1]. Some well-known members of this 𝛼-family are •𝛼 Method • 0 forward difference; forward Euler • 1⁄2 midpoint rule; Crank-Nicolson • 2⁄3 Galerkin • 1 backward difference, fully implicit 35.2 Thermal Boundary Conditions Boundary conditions are represented by LS-DYNA Theory Manual Heat Transfer 𝑘𝑥 ∂𝜃 ∂𝑥 𝑛𝑥 + 𝑘𝑦 ∂𝜃 ∂𝑦 𝑛𝑦 + 𝑘𝑧 ∂𝜃 ∂𝑧 𝑛𝑧 = 𝛾 − 𝛽𝜃 = 𝑞′′̇ . (35.7) By convention, heat flow is positive in the direction of the surface outward normal vector. Surface definition is in accordance with the right hand rule. The outward normal vector points to the right as one progresses from node N1 to N2 to N3 and finally to N4. See Figure 35.1. Boundary conditions can be functions of temperature or time. More than one boundary condition can be specified over the same surface such as in a case of combined convection and radiation. For situations where it is desired to specify adiabatic (i.e., 𝑞′′̇ = 0) conditions, such as at an insulated surface or on a line of symmetry, no boundary condition need be specified. This is the default boundary condition in LS-DYNA. Temperature boundary condition can be specified on any node whether on the physical boundary or not. Flux, convection, and radiation boundary conditions are specified on element surface segments defined by 3 (triangular surface) or 4 nodes (quadrilateral surface). These boundary conditions can be specified on any finite element surface whether on the physical boundary or not. • Flux: Set 𝑞′′̇ = 𝑞𝑓 , where 𝑞𝑓 is defined at the node points comprising the flux boundary condition surface. • Convection: A convection boundary condition is calculated using 𝑞′′̇ = ℎ(𝑇 − 𝑇∞), where ℎ is heat transfer coefficient, (𝑇 − 𝑇∞) is temperature potential. LS- DYNA evaluates ℎ at the film temperature N1 N4 N3 N2 Figure 35.1. Definition of the outward normal vector Heat Transfer LS-DYNA Theory Manual 𝑇 = (𝑇surf + 𝑇∞) (35.8) • Radiation: A radiation boundary condition is calculated using 𝑞′′̇ = ℎ 𝑟(𝑇4 − 4 ), where ℎ 𝑟 = 𝜎𝜀𝐹 is a radiant-heat-transfer coefficient. 𝑇∞ 35.3 Thermal Energy Balances Various energy terms are printed and written into the plot file for post processing using the code LS-PREPOST. The energy terms are: • • • • • change in material internal energy for time step, change in material internal energy from initial time, heat transfer rates on boundary condition surfaces, heat transfer rates on enclosure radiation surfaces, 𝑥, 𝑦, and 𝑧 fluxes at all nodes. 35.4 Heat Generation Volumetric heat generation rates may be specified by element, by material, or both (in which case the effect is additive). Volumetric heat generation rates can be a function of time or temperature. 35.5 Initial Conditions Initial temperature conditions can be specified on the nodal data input cards or on the nodal temperature initial condition cards. If no temperatures are specified, the default is 0. For nonlinear steady state problems the temperature initial condition serves as a first guess for the equilibrium iterations. 35.6 Material Properties Heat capacity and thermal conductivity may be functions of temperature. Since the density and heat capacity appear only as a product in the governing equations, the LS-DYNA Theory Manual Heat Transfer temperature dependence of the density may be included in the temperature dependence of the heat capacity. Material properties are evaluated at the element Gauss point temperature or average element temperature. The thermal conductivity may be either isotropic or orthotropic. For an orthotropic material, the three material axes (𝑥′1, 𝑥′2, 𝑥′3) are orthogonal and the thermal conductivity tensor 𝐊 is diagonal. The thermal conductivity tensor 𝐊 in the global coordinate system is related by where 𝐾𝑖𝑗 = 𝐾′𝑖𝑗𝛽𝑚𝑖𝛽𝑛𝑗, 𝛽𝑖𝑗 = cos(𝑥′𝑖, 𝑥𝑗). (35.9) (35.10) 35.7 Nonlinear Analysis In a nonlinear problem, 𝐶, 𝐻, and 𝐹 are functions of temperature. Newton’s method is used to transform equation 32.4 into an alternate form which contains temperature derivatives of 𝐶, 𝐻, and 𝐹 (i.e., the tangent matrix). Iterations are required to solve this alternate form. In a steady state nonlinear problem, an initial guess should be made of the final temperature distribution and included in the input file as an initial condition. If your guess is good, a considerable savings in computation time is achieved. 35.8 Units Any consistent set of units with the governing equation may be used. Examples are: Quantity temperature space time density heat capacity thermal conductivity thermal generation Units K m s kg/m3 J/kg k W/m K W/M3 F C ft cm hr s Lbm/ft3 g/cm3 cal/g c Btu/LbmF cal/s cm C Btu/hr ft F Btu/hr ft3 cal/s cm3 Heat Transfer LS-DYNA Theory Manual heat flux W/m2 cal/s cm2 Btu/hr ft2 LS-DYNA Theory Manual Adaptivity 36 Adaptivity LS-DYNA includes an h-adaptive method for the shell elements. In an h-adaptive method, the elements are subdivided into smaller elements wherever an error indicator shows that subdivision of the elements will provide improved accuracy. An example of an adaptive calculation on a thin wall square cross section beam is shown in Figure 36.1. In Figures 36.2 through 36.4 a simple metal stamping simulation is shown [also see Galbraith, Finn, et. al., 1991]. In the following, the methodologies used in the h-adaptive method in LS-DYNA are described. The objective of the adaptive process used in LS-DYNA is to obtain the greatest accuracy for a given set of computational resources. The user sets the initial mesh and the maximum level of adaptivity, and the program subdivides those elements in which the error indicator is the largest. Although this does not provide control on the error of the solution, it makes it possible to obtain a solution of comparable accuracy with fewer elements, and, hence, less computational resources, than with a fixed mesh. LS-DYNA uses an h-adaptive process, where parts of the mesh are selectively refined during the course of the solution procedure. The methodology used is based on Belytschko, Wong, and Plaskacz [1989]. In the former, elements were also fused or combined when it was felt that they were no longer needed. It was found that the implementation of fusing procedures for general meshes, such as occur in typical applications of commercial programs, is too complex, so only fission is included. Adaptivity in LS-DYNA can be restricted to specific groups of shell elements. Elements that fall in this group are said to be in the active adaptivity domain. Adaptivity LS-DYNA Theory Manual Figure 36.1. One level adaptive calculation on a square cross section beam. Figure 36.2. Aluminum blank with 400 shells in blank and four rigid tools. LS-DYNA Theory Manual Adaptivity Figure 36.3. Adaptive calculations using two adaptive levels. In the h-adaptive process, elements are subdivided into smaller elements where more accuracy is needed; this process is called fission. The elements involved in the fission process are subdivided into elements with sides ℎ/2, where ℎ is the characteristic size of the original elements. This is illustrated in Figure 36.5 for a quadrilateral element. In fission, each quadrilateral is subdivided into four quadrilaterals (as indicated in Figure 36.2) by using the mid-points of the sides and the centroid of the element to generate four new quadrilaterals. Figure 36.4. Final shape of formed part with 4315 shell elements per quarter. Adaptivity LS-DYNA Theory Manual Figure 36.5. Fissioning of a Quadrilateral Element The fission process for a triangular element is shown in Figure 36.6 where the element is subdivided into four triangles by using the mid-points of the three sides. The adaptive process can consist of several levels of fission. Figure 36.5 shows one subdivision, which is called the second refinement level. In subsequent steps, the fissioned elements can again be fissioned in a third refinement level, and these elements can again, in turn, be fissioned in a fourth level, as shown in Figure 36.7. The levels of adaptivity that occur in a mesh are restricted by three rules: • The number of levels is restricted by the maximum level of adaptivity that is allowed in the mesh, which is generally set at 3 or 4. At the fourth level up to 64 elements will be generated for each element in the initial mesh. • The levels of adaptivity implemented in a mesh must be such that the levels of adaptivity implemented in adjacent elements differ by, at most, one level. • The total number of elements can be restricted by available memory. Once the specified memory usage is reached, adaptivity ceases. The second rule is used to enforce a 2-to-1 rule given by Oden, Devloo and Strouboulis [1986], which restricts the number of elements along the side of any element in the mesh to two. The enforcement of this rule is necessary to accommodate limitations in the data structure. The original mesh provided by the user is known as the parent mesh, the elements of this mesh are called the parent elements, and the nodes are called parent Figure 36.6. Fissioning of a Triangular Element nodes. Any elements that are generated by the adaptive process are called descendant LS-DYNA Theory Manual Adaptivity Figure 36.7. Quadrilateral Element Fissioned to the fourth level elements, and any nodes that are generated by the adaptive process are called descendant nodes. Elements generated by the second level of adaptivity are called first- generation elements, those generated by third level of adaptivity are called second- generation elements, etc. The coordinates of the descendant nodes are generated by using linear interpolation. Thus, the coordinates of any node generated during fission of an element are given by 𝑥𝑁 = (𝑥𝐼 + 𝑥𝐽), (36.1) where 𝑥𝑁 is the position of the generated node and 𝑥𝐼 and 𝑥𝐽 are the nodes along the side on which 𝑥𝑁 was generated for a typical element as shown in Fig. 33.1. The coordinate of the mid-point node, which is generated by fission of a quadrilateral element, is given by 𝑥𝑀 = (𝑥𝐼 + 𝑥𝐽 + 𝑥𝐾 + 𝑥𝐿), (36.2) where 𝑥𝑀 is the new midpoint node of the fissioned quadrilateral and 𝑥𝐼, 𝑥𝐽, 𝑥𝐾 and 𝑥𝐿 are the nodes of the original quadrilateral. The velocities of the nodes are also given by linear interpolation. The velocities of edge nodes are given by and the angular velocities are given by 𝑣𝑁 = (𝑣𝐼 + 𝑣𝐽), 𝜔𝑁 = (𝜔𝐼 + 𝜔𝐽). The velocities of a mid-point node of a fissioned quadrilateral element are given by 𝑣𝑀 = (𝑣𝐼 + 𝑣𝐽 + 𝑣𝐾 + 𝑣𝐿), 𝜔𝑀 = (𝜔𝐼 + 𝜔𝐽 + 𝜔𝐾 + 𝜔𝐿). (36.3) (36.4) (36.5) (36.6) Adaptivity LS-DYNA Theory Manual out-of-plane undeformed deformed Figure 36.8. Refinement indicator based on angle change. The stresses in the descendant element are obtained from the parent element by setting the stresses in the descendant elements equal to the stresses in the parent element at the corresponding through-the-thickness quadrature points. In subsequent steps, nodes which are not corner nodes of an all attached elements are treated as slave nodes. They are handled by the simple constraint equation. Refinement indicators are used to decide the locations of mesh refinement. One deformation based approach checks for a change in angles between contiguous elements as shown in Figure 36.8. If 𝜁 > 𝜁tol then refinement is indicated, where 𝜁tol is user defined. LS-DYNA Theory Manual Adaptivity Figure 36.9. The input parameter, ADPASS, controls whether LS-DYNA backs up and repeats the calculation after adaptive refinement. After the mesh refinement is determined, we can refine the mesh and continue the calculation or back up to an earlier time and repeat part of the calculation with the new mesh. For accuracy and stability reasons the latter method is generally preferred; however, the former method is preferred for speed. Whether LS-DYNA backs up and repeats the calculation or continues after remeshing is determined by an input parameter, ADPASS. This is illustrated in Figure 36.9. LS-DYNA Theory Manual Implicit 37 Implicit 37.1 Introduction Implicit solvers are properly applied to static, quasi-static, and dynamic problems with a low frequency content. Such applications include but are not limited to • Static and quasi-static structural design and analysis • Metal forming, especially, the binderwrap and springback • Gravitational loading of automotive structures • Linear buckling and vibration analysis An advantage of the implicit solver on explicit integration is that the number of load or time steps is typically 100 to 10000 times fewer. The major disadvantage is that the cost per step is unknown since the speed depends mostly on the convergence behavior of the equilibrium iterations which can vary widely from problem to problem. An incremental-iterative numerical algorithm is implemented in LS-DYNA. The method is stable for wide range of nonlinear problems that involve finite strain and arbitrarily large rotations. Accuracy consideration usually limits the load increment or time step size. An inaccurate solution will often not converge. Nine iterative schemes are available including the full Newton method and eight quasi-Newton methods. These are: • Full Newton, • BFGS (default), • Broyden, • Davidon-Fletcher-Powell (DFP) [Schweizerhof 1986], • Davidon symmetric, [Schweizerhof 1986], • modified constant arc length with BFGS, Implicit LS-DYNA Theory Manual • modified constant arc length with Broyden’s, • modified constant arc length with DFP, • modified constant arc length with Davidon. A line search is combined with each of these schemes along with automatic stiffness reformations, as needed, to avoid non-convergence. LS-DYNA defaults to the BFGS quasi-Newton method which is the most robust although the other methods are sometimes superior. Generally, the quasi-Newton methods require fewer iterations than the modified Newton method since they exhibit superlinear local convergence due to the rank one or rank two updates of the stiffness matrix as the iterations proceed. In this chapter, important aspects of the static and dynamic algorithm are explained, hopefully, in a way that will be understandable to all users. The arc length methods are generally used in solving snap through buckling problems and details on one specific implementation is taken up in the next chapter. 37.2 Equations 37.2.1 Discretization Neglecting constraints, discretization formally leads to the matrix equations of motion 𝑹 = 𝑴𝒙̈ + 𝑭𝑖 − 𝑭𝑒 = 𝟎 (37.1) where 𝒙̈ = acceleration vector of length 𝑛 𝑴 = 𝑛 × 𝑛 mass matrix 𝑭𝑒 = body force and external load vector of length 𝑛 𝑭𝑖 = internal force vector of length 𝑛. It is implicitly assumed that the involved vectors 𝑭𝑖 and 𝑭𝑒 depend on6 𝒙̇, 𝒙 = velocity and coordinate vectors of length 𝑛 𝑡 = simulation time as well as on some history of the deformation, while 𝑴 is constant. In practice, the only independent variable is 𝒙 since the velocity 𝒙̇ and acceleration 𝒙̈ are typically expressed in terms of this coordinate vector by the time integration scheme used, and 𝑡 is given. Deformation history is typically accounted for in internal variables associated with features in the model, such as plastic strains in materials and frictional sliding in contacts. 6 This is true prior to time discretization, vectors 𝑭(cid:3036) and 𝑭(cid:3032) depend on 𝒙 and on 𝒙(cid:4662) only through the exact time differentiation. Once time discretization is done according to some scheme, the dependence is on 𝒙 and not necessarily on the discretized 𝒙(cid:4662) but rather ∆𝒙/∆𝑡, see Section 1.4.1. LS-DYNA Theory Manual Implicit A diagonal lumped mass matrix is obtained by row summing according to 𝑀𝑖𝑖 = ∫ 𝜌𝜙𝑖 ∑ 𝜙𝑗 𝑑𝑉 = ∫ 𝜌𝜙𝑖𝑑𝑉 (37.2) where 𝜌 is material density and 𝑉 denotes the body over which integration occurs. The primary nonlinearities, which are due to geometric effects and inelastic material behavior, are accounted for in 𝑭𝑖, 𝑭𝑖 = ∫ 𝑩𝑇𝝈𝑑𝑉 , (37.3) where 𝑩 is the strain-displacement matrix and 𝝈 is the stress. Additional nonlinearities arise in 𝑭𝑒 due to geometry dependent applied loads, such as contacts and loads on segments. Explicit integration trivially satisfies (37.1) since the calculation of the acceleration guarantees equilibrium, i.e., from time step 𝑗 to 𝑗 + 1 we use 𝒙̈𝑗 = 𝑴 −1[𝑭𝑒 𝑗 − 𝑭𝑖 𝑗]. The explicit update of the velocities and coordinates is given by 𝒙̇ 𝑗+1/2 = 𝒙̇ 𝑗−1/2 + 𝛥𝑡𝑗𝒙̈𝑗, 𝒙𝑗+1 = 𝒙𝑗 + 𝛥𝑡𝑗+1/2𝒙̇𝑗+1/2. (37.4) (37.5) (37.6) Stability places a limit on the time size. This step size may be very small and, consequently, a large number of steps may be required. Implicit analysis employs schemes that are unconditionally stable, thus allowing for larger steps at the cost of a more expensive update of the geometry. 37.2.2 Constraints Constraints is obviously an important ingredient in nonlinear finite elements, and may include for instance simple point or motion constraints, slave nodes constrained to rigid bodies, joints and tied contacts. Constraints are divided into two categories, those that are directly eliminated (first kind) and those that are treated with Lagrangian multipliers 𝝀 (second kind). The principle behind (37.1) is that of virtual work, stating that 𝛿𝒙𝑇(𝑹 + 𝑪𝜆 𝑇𝝀) = 0 (37.7) for any admissible virtual displacement field 𝛿𝒙. Admissible displacement fields are those that satisfy the first kind of constraints. The second kind is instead treated by the Implicit LS-DYNA Theory Manual second term inside the parenthesis, for which we require satisfaction of 𝑚𝜆 additional constraints 𝑯𝜆(𝒙, 𝑡) = 𝟎 (37.8) and 𝜕𝑯𝜆 𝜕𝒙 If there are no constraint of the first kind, any displacement field is admissible and 𝑇𝝀 = 𝟎. The presence of first kind constraints put restrictions on 𝛿𝒙 and the hence 𝑹 + 𝑪𝜆 following is an attempt to derive the proper nonlinear equations in this context. 𝑪𝜆 = (37.9) . Constraints of the first kind augment the 𝑛 equations of motion by imposing 𝑚 additional equations and consequently (37.1) is to be reduced to 𝑛 − 𝑚 equations. To this end, we introduce the 𝑚 × 𝑛 constraint matrix 𝑯(𝒙, 𝑡) = 𝟎, (37.10) 𝑪 = 𝜕𝑯 𝜕𝒙 , (37.11) and conveniently partition the global vector 𝒙 into an independent (solution) part 𝒙𝐼 of length 𝑛 − 𝑚 and dependent part 𝒙𝐷 of length 𝑚. This partitioning is represented by projection matrices 𝑷𝐼 and 𝑷𝐷 such that and 𝒙𝐼 = 𝑷𝐼𝒙, 𝒙𝐷 = 𝑷𝐷𝒙 𝒙 = 𝑷𝐼 𝑇𝒙𝐼 + 𝑷𝐷 𝑇 𝒙𝐷, (37.12) (37.13) and the space of admissible virtual displacements is that of any 𝛿𝒙𝐼. The criterion for a valid partitioning is that the 𝑚 × 𝑚 matrix given by 𝑇 , 𝑪𝐷 = 𝑪𝑷𝐷 (37.14) is non-singular, which is always possible unless there are conflicting or redundant constraints. The Linear Constraint PACKage (LCPACK) in LS-DYNA performs this partitioning and invalid constraints will result in error termination. Introducing the 𝑚 × (𝑛 − 𝑚) matrix we can combine the variations of (37.10) and (37.13) and use (37.14) and (37.15) to obtain 𝑪𝐼 = 𝑪𝑷𝐼 (37.15) 𝛿𝒙 = 𝑷𝑇𝛿𝒙𝐼, (37.16) where LS-DYNA Theory Manual Implicit 𝑇𝑪𝐷 is a projection-like matrix from the global variable space to the independent solution space. Using this expression for 𝛿𝒙 in the principle of virtual work (37.7), the arbitrariness of 𝛿𝒙𝐼 results in 𝑷 = 𝑷𝐼 − 𝑪𝐼 −𝑇𝑷𝐷 (37.17) with 𝑸 = 𝟎, 𝑸 = 𝑷(𝑹 + 𝑪𝜆 𝑇𝝀). (37.18) (37.19) This can be interpreted as to solve for zero force in the direction of deformation that is not constrained, in other directions the constraints induce reaction forces that are typically monitored in the LS-DYNA ascii and binout databases associated with the constraint type. The reaction forces corresponding to those constraints of the second kind is contained in 𝝀. 37.2.3 Reaction forces due to constraints Alternatively, we may form the lagrangian ℒ for the entire system as ℒ(𝒙, 𝝀, 𝑡) = ℇ(𝒙, 𝑡) + 𝝀𝑇𝑯(𝒙, 𝑡) (37.20) where ℇ is an assumed potential for the residual force 𝑹. It is important to stress that the potential may not exist in general, this requires that the system is conservative in the sense of e.g. hyperelasticity. But it serves the purpose here for deriving the Lagrangian multiplier 𝝀 and subsequently the reaction forces due to the constraints 𝑯. The Karush- Kuhn-Tucker conditions for equilibrium is now (omitting arguments) 𝑹 + 𝑪𝑇𝝀 = 𝟎 = 𝟎 (37.21) where 𝝀 is a vector of length 𝑚 to be interpreted as the resisting force needed to maintain the constraints. Continuing, we split 𝑹 and 𝑪 into their respective independent and dependent parts, leading to a rewrite of the first of (37.21) 𝑹𝐼 + 𝑪𝐼 𝑹𝐷 + 𝑪𝐷 𝑇𝝀 = 𝟎 𝑇 𝝀 = 𝟎 (37.22) from which the Lagrangian multipliers can be solved from the second of (37.22) as 𝝀 = −𝑪𝐷 −𝑇𝑹𝐷. (37.23) This is the (generalized) force needed to enforce the second of (37.21). To obtain the corresponding nodal (reaction) force vector associated with a single constraint 𝑗 ∈ [1, 𝑚] we form Implicit LS-DYNA Theory Manual 𝒓𝑗 = 𝜆𝑗𝒄𝑗 (37.24) where 𝒄𝑗 is the 𝑗:th row in the constraint matrix 𝑪, and 𝜆𝑗 is the corresponding component of 𝝀. These are the equations that form the basis for the detailed database outputs, such as bndout in the case of prescribed motion. 37.3 Implicit Statics 37.3.1 Linearization For the implicit static solution 𝑴 = 𝟎 in (37.1) and the residual and constraint vector at a given time 𝑡 becomes an implicit function of 𝒙 only. We seek the vector 𝒙 and multiplier 𝝀 such that (37.8) and (37.10) holds together with 𝑸(𝒙, 𝝀) = 𝟎. (37.25) Assume an approximation 𝒙𝑘 to 𝒙 and 𝝀𝑘 to 𝝀 for 𝑘 = 1, 2, 3...etc. In the neighborhood of 𝒙𝑘 and 𝝀𝑘 we use a linear approximation to (37.10) and (37.25) given by 𝑘 + 𝑷𝑪𝜆 𝑇𝛥𝝀𝑘 = 𝑭(𝒙𝑘, 𝝀𝑘), 𝑲(𝒙𝑘)𝛥𝒙𝐼 (37.26) and iterate for the solution 𝑘+1 = 𝒙𝐼 𝒙𝐼 𝑘, 𝑘 + 𝑠𝛥𝒙𝐼 𝝀𝑘+1 = 𝝀𝑘 + 𝑠𝛥𝝀𝑘 (37.27) Here 𝑠 is a convenient step size to be discussed below, as will be the update of the 𝑘+1. The linear system (37.26) is derived using the assumption that 𝑷 is dependent part 𝒙𝐷 independent of 𝒙, which is generally not true. Many constraints in LS-DYNA are nonlinear and a strict linearization would have to take the second variation of constraints into account. But this would be inherently complex, thus linearizing (37.25) using (37.19) just becomes 𝑸(𝒙𝑘+1, 𝝀𝑘+1) ≈ 𝑸(𝒙𝑘, 𝝀𝑘) + 𝑷 𝜕𝑹 𝜕𝒙 To be able to solve for ∆𝒙𝑘 and Δ𝝀𝑘 this needs first to be combined with a linearized equation of the constraint (37.10) (𝒙𝑘)∆𝒙𝑘 + 𝑷𝑪𝜆 𝑇𝛥𝝀𝑘 = 𝟎. (37.28) 𝑯(𝒙𝑘+1) ≈ 𝑯(𝒙𝑘) + 𝑪(𝒙𝑘)∆𝒙𝑘 = 𝟎, (37.29) and an incremental correspondent to (37.13) 𝑘 + 𝑷𝐷 These last two equations together with (37.14) and (37.15) can be used to yield an expression for the dependent part of the displacement increment ∆𝒙𝑘 = 𝑷𝐼 𝑘 . 𝑇 ∆𝒙𝐷 𝑇∆𝒙𝐼 (37.30) −1(𝒙𝑘)[𝑯(𝒙𝑘) + 𝑪𝐼(𝒙𝑘)∆𝒙𝐼 Using (19.22) in (37.30) in (37.28) results in expressions of the vector 𝑭 and jacobian 𝑲 in (37.26) as 𝑘 = −𝑪𝐷 (37.31) ∆𝒙𝐷 𝑘]. LS-DYNA Theory Manual 𝑭(𝒙𝑘, 𝝀𝑘) = −𝑸(𝒙𝑘, 𝝀𝑘) + 𝑷 𝜕𝑹 𝜕𝒙 and (𝒙𝑘)𝑷𝐷 𝑇 𝑪𝐷 −1(𝒙𝑘)𝑯(𝒙𝑘) 𝑲(𝒙𝑘) = 𝑷 𝜕𝑹 𝜕𝒙 (𝒙𝑘)𝑷𝑇. Implicit (37.32) (37.33) The dependent part of the solution vector is in general analogous to (37.27) of the indendent part 𝑘 + 𝑠∆𝒙𝐷 except for those constraint equations where there is an explicit expression 𝒙𝐷 = 𝒙𝐷(𝒙𝐼), then of course 𝑘+1 = 𝒙𝐷 𝒙𝐷 (37.34) 𝑘+1 = 𝒙𝐷(𝒙𝐼 𝒙𝐷 𝑘+1). (37.35) The constraint vector corresponding to those of the second kind needs also to be linearized, 𝑯𝜆(𝒙𝑘+1) ≈ 𝑯𝜆(𝒙𝑘) + 𝑪𝜆(𝒙𝑘)∆𝒙𝑘 = 𝟎, (37.36) and repeating the same procedure as above, we are lead to 𝑪𝜆(𝒙𝑘)𝑷𝑇∆𝒙𝐼 𝑘 = 𝑮(𝒙𝑘) with 𝑮(𝒙) = −𝑯𝜆(𝒙) + 𝑪𝜆(𝒙)𝑷𝐷 𝑇 𝑪𝐷 −1(𝒙)𝑯(𝒙), (37.37) (37.38) which completes the linearization. In sum, the Newton step thus means solving the combined system (37.26) and (37.37) for ∆𝒙𝑘 and ∆𝝀𝑘 and update the solution using (37.27). For simplicity, we will hereforth assume 𝑚𝜆 = 0, i.e., all constraints are of the first kind, to simplify the exposition. from The jacobian matrix 𝑲 is the assembly of the tangent moduli of materials, external loads, contacts, etc., and is in practice only an approximation due to the complexity of taking all dependencies into account. In particular it does not include the geometric stiffness contribution on CON- TROL_IMPLICIT_GENERAL. A speculative reason is that this has a smoothing effect and eliminates negative eigenvalues due to compressive stresses. If the deformation mode is known to be mainly in tension or if the material is hyper-elastic, including the geometric stiffness could improve convergence however. Often the stiffness matrix is assumed symmetric and positive definite, but is not limited to those characteristics. internal default, forces IGS see by Implicit LS-DYNA Theory Manual Note also that (37.32) indicates that both 𝑸 and 𝑯 must vanish to render a zero 𝑭, thus a zero displacement increment ∆𝒙 in the iterative scheme. Figure 3737-1 Linear axial buckling of an aluminium beverage can. 37.3.2 Linear theory For a linear solution, (37.26) is solved once to obtain the linear displacement vector 𝒖 = ∆𝒙, and often the following assumptions apply. The configuration 𝒙 to which the linear approximation apply is stress free and all constraints are fulfilled, so the right hand side 𝑭 in (37.32) is essentially the external applied load 𝑭𝑒, 𝑭 = 𝑷𝑭𝑒, which is constant. Furthermore, 𝑷 is constant due to trivial constraints and the stiffness matrix 𝑲 in (37.33) thus evaluates from the linearization of internal forces 𝑲 = 𝑷 ∫ 𝑩𝑇𝑬𝑩𝑑𝑉 𝑷𝑇, (37.39) 𝜕𝜺 to denote the constitutive matrix. So in more conventional where we used 𝑬 = 𝜕𝝈 terms, the linear equation is written 𝑲𝒖 = 𝑭. (37.40) Once solved, the stress 𝝈 = 𝑬𝑩𝒖 (37.41) can be evaluated from the constitutive law for the resulting deformation. The stiffness matrix 𝑲 in (37.40) is symmetric and positive definite if 𝑬 is and 𝑷 eliminates all rigid body modes, whence the solution 𝒖 is unique. Furthermore, linearity implies that substituting the right hand side for 𝑭𝜆 = 𝜆𝑭, the solution changes to 𝒖𝜆 = 𝜆𝒖 and the resulting stress changes to linear A TROL_IMPLICIT_SOLUTION. solution is 𝝈𝜆 = 𝜆𝝈. by obtained putting NSOLVR = 1 (37.42) on CON- LS-DYNA Theory Manual Implicit Now go back to the nonlinear static equation and scale a constant external load 𝑭𝑒 with 𝜆 (37.43) and assume an updated configuration 𝒙𝜆 with resulting stress 𝝈𝜆 to be the solution. To see how the solution changes with 𝜆 we can perturb (37.43) to obtain 𝑷[𝑭𝑖 − 𝜆𝑭𝑒] = 𝟎 𝑷 [ 𝜕𝑭𝑖 𝜕𝒙 𝑷𝑇𝛿𝒙𝜆 − 𝛿𝜆𝑭𝑒] = 𝟎 (37.44) where we applied (37.16). This is conveniently rewritten as (37.45) where the presence of stress will change the evaluation of the stiffness matrix from that in (37.39) to 𝑲𝜆𝛿𝒙𝜆 = 𝛿𝜆𝑭, 𝑲𝜆 = 𝑲 + 𝑷 ∫ 𝓑 𝑇𝝈𝜆𝓑𝑑𝑉 𝑷𝑇. (37.46) Here the second term is the geometric contribution to the tangent stiffness matrix where 𝓑 is a matrix consisting of shape function derivatives for the finite element. We are interested in the question of uniqueness of 𝛿𝒙𝜆 as the solution to (37.45), and this uniqueness is lost when (37.47) If one assumes that deformations are small enough to keep 𝑉, 𝑩, 𝑬 and 𝓑 independent of 𝜆, and that (37.42) holds with (37.41) and (37.40), then (37.47) can be stated as the following eigenvalue problem det(𝑲𝜆) = 0. with the geometric (nonlinear) stiffness matrix given by 𝑲𝛿𝒖 = −𝜆𝑲𝜎𝛿𝒖 𝑲𝜎 = 𝑷 ∫ 𝓑 𝑇𝝈𝓑𝑑𝑉 𝑷𝑇 (37.48) (37.49) and 𝑲 is the material (linear) stiffness matrix again given by (37.39). This is the theory behind linear buckling, see CONTROL_IMPLICIT_BUCKLE, with 𝜆 being the buckling load parameter and 𝛿𝒖 the associated buckling mode. Usually solutions with 𝜆 > 0 are of interest, and from (37.48) and (37.49) it then follows that the principal stresses cannot be positive throughout the domain of integration. In other words, the model must somehow be in a compressed state. The full procedure is 1.Assemble 𝑲 by (37.39). 2.Solve (37.40) for a constant reference load 𝑭. 3.Evaluate resulting stress 𝝈 by (37.41). 4.Assemble 𝑲𝜎 by (37.49). 5.Solve (37.48) for 𝜆 and 𝛿𝒖. An example of linear buckling is shown in Figure 3737-1, simulating the stepping on an aluminium beverage can. Implicit LS-DYNA Theory Manual 𝐹 𝐹0 𝐹0 𝐹1 𝐹2 𝑥2 𝑥1 𝑥0 𝐹1 𝐹2 𝑥2 𝑥1 𝑥0 Figure 3737-2 Full Newton (left) compared to quasi-Newton secant updates (right), the linear approximation to obtain 𝑥2 is for full Newton the exact tangent in (𝑥1, 𝐹1) while it is the linear extension between the points (𝑥0, 𝐹0) 37.3.3 Quasi-Newton iterations Now back to the nonlinear theory. To obtain the solution at load increment 𝑗 + 1 given the solution at load increment 𝑗, linearized equations of the form 𝑲𝑘𝛥𝒙𝑘 = 𝑭𝑘, (37.50) are assembled and solved where 𝑘 is the iteration number and 𝑲𝑘 = Tangent stiffness matrix Δ𝒙𝑘 = Desired increment in displacements 𝑭𝑘 = Residual load vector. This should be seen a generalization of (37.26) in the sense that the tangent stiffness matrix 𝑲 need not be calculated as (37.33) but can be based on other approximations to be presented. We do however assume, without loss of generality, that (37.50) is in the independent system of variables so the residual vector 𝑭 is given by (37.32). We here just substitute the sub-index 𝐼 in the incremental displacement ∆𝒙 for the iteration counter 𝑘 to simplify the notation in the following. The coordinate vector is updated 𝒙𝑘+1 = 𝒙𝑘 + sΔ𝒙𝑘, (37.51) where 𝑠 is a parameter between 0 and 1 found from a line search. If the tangent stiffness matrix is calculated as (37.33) for each 𝑘 then this is termed a full Newton method, but it may be beneficial to use so called quasi-Newton updates of 𝑲−1 to avoid the cost of solving a linear system of equations in each iteration. Four such methods for updating the stiffness matrix are available • Broyden’s first method LS-DYNA Theory Manual Implicit • Davidon • DFP • BFGS and these involve rank 1 or rank 2 stiffness updates. Quasi-Newton methods are less expensive than the full Newton method but often still result in robust program. In one dimension, quasi-Newton corresponds to secant iterations and this method compared to full Newton is illustrated in Figure 3737-2. Henceforth we assume that 𝑲0 represents the last assembled matrix according to (37.33) and then 𝑲𝑘, 𝑘 = 1,2,3, … are quasi- Newton updates to be given in the following. The secant matrices 𝑲𝑘 are found via the quasi-Newton equations where 𝑲𝑘Δ𝒙𝑘−1 = Δ𝑭𝑘, Δ𝑭𝑘 = 𝑭𝑘−1 − 𝑭𝑘. (37.52) (37.53) Two classes of matrix updates that satisfy the quasi-Newton equations are of interest; rank 1 updates and rank 2 updates 𝑲𝑘 = 𝑲𝑘−1 + 𝛼𝒛𝒚𝑇, 𝑲𝑘 = 𝑲𝑘−1 + 𝛼𝒛𝒚𝑇 + 𝛽𝒗𝒖𝑇. Substituting (37.54) into (37.52) gives 𝑲𝑘−1𝛥𝒙𝑘−1 + 𝛼𝒛𝒚𝑇𝛥𝒙𝑘−1 = 𝛥𝑭𝑘. (37.54) (37.55) (37.56) By choosing 𝛼 = 1 𝒚𝑇𝛥𝒙𝑘−1 arbitrary vector but is restricted such that and 𝒛 = −𝑭𝑘, equation (37.52) is satisfied. Note that 𝒚 is an The tangent stiffness update is 𝒚𝑇𝛥𝒙𝑘−1 ≠ 0. 𝑲𝑘 = 𝑲𝑘−1 − 𝑭𝑘𝒚𝑇 𝒚𝑇𝛥𝒙𝑘−1 , (37.57) (37.58) resulting generally in non-symmetric secant matrices. The inverse forms are found by the Sherman-Morrison formula (𝑨 + 𝒂𝒃𝑇) −1 = 𝑨−1 − 𝑨−1𝒂 𝒃𝑇𝑨−1 1 + 𝒃𝑇𝑨−1𝒂 . (37.59) where 𝑨 is a nonsingular matrix and 𝒂 and 𝒃 are arbitrary vectors such that 1 + 𝒃𝑇𝑨−1𝒂 ≠ 0. The inverse form for (37.58) can be found by letting 𝑨 = 𝑲𝑘−1, 𝒂 = −𝑭𝑘 𝒚𝑇𝛥𝒙𝑘−1 , 𝒃 = 𝒚, (37.60) Implicit LS-DYNA Theory Manual in the Sherman-Morrison formula. Therefore, 𝑲𝑘 −1 = [𝑲𝑘−1 ⎢⎡𝑰 + ⎣ −1 𝑭𝑘]𝒚𝑇 𝒚𝑇𝛥𝑭𝑘 Broyden´s method use 𝒚 = ∆𝒙𝑘−1 resulting in non-symmetric stiffness updates, and an algorithm for this exploits that 𝒅𝑘∆𝒙𝑘−1 𝛾𝑘 𝒅𝑘−1∆𝒙𝑘−2 𝛾𝑘−1 𝒅1∆𝒙0 𝛾1 ⎥⎤ 𝑲𝑘−1 −1 . ⎦ −1 = [𝑰 + ] … [𝑰 + ] [𝑰 + ] 𝑲0 −1 𝑲𝑘 (37.61) (37.62) where (37.63) To illustrate the efficiency of a quasi-Newton method we outline the steps to obtain ∆𝒙𝑘. 1.Assume ∆𝒙0, 𝑭𝑘 and 𝑭𝑘−1 (recalling (37.53)) are known, as well as ∆𝒙𝑖, 𝒅𝑖 and 𝛾𝑖 for 𝛾𝑘 = ∆𝒙𝑘−1 𝒅𝑘 = 𝑲𝑘−1 𝑇 ∆𝑭𝑘. −1 𝑭𝑘, 𝑖 = 1, … , 𝑘 − 1. −1𝑭𝑘. 2.Solve 𝒆0 = 𝑲0 3.Recursively compute 𝒆𝑖 = 𝒆𝑖−1 + 𝑇 ∆𝑭𝑘. 4.Set 𝒅𝑘 = 𝒆𝑘−1 and 𝛾𝑘 = ∆𝒙𝑘−1 𝑇 𝒅𝑘 ∆𝒙𝑘−1 ] 𝒅𝑘. 5.Compute ∆𝒙𝑘 = [1 + 𝛾𝒌 𝑇 𝒆𝑖−1 ∆𝒙𝑖−1 𝛾𝒊 𝒅𝑖 for 𝑖 = 1, … , 𝑘 − 1. Noteworthy here is that an iteration consists of a forward and backward substitution of an already factorized matrix (step 2) plus a sequence of vector operations (steps 3-5), which altogether presumably is much less expensive than solving an entire system of linear equations. The algorithm requires an in-core storage consisting of 2𝑘 vectors and 𝑘 scalars to complete iteration 𝑘. Again, recalling the quasi-Newton equation (37.52), and substituting (37.55) gives 𝑲𝑘−1𝛥𝒙𝑘−1 + 𝛼𝒛𝒚𝑇𝛥𝒙𝑘−1 + 𝛽𝒗𝒖𝑇𝛥𝒙𝑘−1 = 𝛥𝑭𝑘, , 𝒛 = −𝑭𝑘−1, 𝛽 = 1 and 𝒗 = 𝛥𝑭𝑘. Here 𝒚 and 𝒖 are arbitrary (37.64) and set 𝛼 = 1 vectors that are non-orthogonal to 𝛥𝒙𝑘−1, i.e., 𝒚𝑇𝛥𝒙𝑘−1 𝒖𝑇𝛥𝒙𝑘−1 and In the BFGS method 𝒚𝑇𝛥𝒙𝑘−1 ≠ 0, 𝒖𝑇𝛥𝒙𝑘−1 ≠ 0. which leads to the following update formula 𝒚 = 𝑭𝑘−1 𝒖 = 𝛥𝑭𝑘, 𝑲𝑘 = 𝑲𝑘−1 + 𝛥𝑭𝑘𝛥𝑭𝑘 𝛥𝒙𝑘−1 𝑇 𝛥𝑭𝑘 − 𝑭𝑘−1𝑭𝑘−1 𝑇 𝑭𝑘−1 𝛥𝒙𝑘−1 , (37.65) (37.66) (37.67) (37.68) that preserves symmetry of the secant matrix. A double application of the Sherman- Morrison formula then leads to the inverse form. LS-DYNA Theory Manual Implicit Special product forms have been derived for the DFP and BFGS updates and exploited by Matthies and Strang [1979], 𝑲𝑘 −1 = [𝑰 + 𝒒𝑘𝒑𝑘 𝑇] 𝑲𝑘−1 −1 [𝑰 + 𝒑𝑘𝒒𝑘 𝑇]. (37.69) The primary advantage of the product form is that the determinant of 𝑲𝑘 and therefore, the change in condition number can be easily computed to control updates. The updates vectors are defined as 𝒑𝑘 = −𝛥𝑭𝑘 − 𝑭𝑘−1√ 𝛥𝒙𝑘−1 𝛥𝒙𝑘−1 𝑇 𝛥𝑭𝑘 𝑇 𝑭𝑘−1 , 𝛥𝒙𝑘−1 𝑇 𝛥𝑭𝑘 Noting that the determinant of 𝑲𝑘 is given by 𝛥𝒙𝑘−1 𝒒𝑘 = . det(𝑲𝑘) = det(𝑲𝑘−1)[1 + 𝒒𝑘 𝑇𝒑𝑘] , it can be shown that the change in condition number, 𝑐, is 𝑐 = [√𝒑𝑘 𝑇𝒑𝑘 𝒒𝑘 𝑇𝒒𝑘 + √𝒑𝑘 𝑇𝒑𝑘 𝒒𝑘 𝑇𝒒𝑘 + 4 (1 + 𝒑𝑘 𝑇𝒒𝑘 )] 𝑇𝒒𝑘)] [4 (1 + 𝒑𝑘 (37.70) (37.71) (37.72) (37.73) . Following the approach of Matthies and Strang [1979] this condition number is used to decide whether or not to do a given update. The quasi-Newton condition (37.52) is easily verified using (37.69) for a real non-singular tangent matrix 𝑲𝑘−1 and it follows that BFGS preserves not only symmetry but also positive definiteness. Interestingly enough the converse is not true; if 𝑲𝑘−1 is indefinite then 𝑲𝑘 may still be positive definite. An algorithm would utilize that 𝑲𝑘 𝑇], 𝑇]𝑲0 −1[𝑰 + 𝒑1𝒒1 𝑇] … [𝑰 + 𝒒1𝒑1 −1 = [𝑰 + 𝒒𝑘𝒑𝑘 𝑇] … [𝑰 + 𝒑𝑘𝒒𝑘 (37.74) −1𝑭𝑘 requires a sequence of vector operations, followed so the computation of ∆𝒙𝑘 = 𝑲𝑘 by a forward and backward substitution of a factorized matrix, followed by yet another sequence of vector operations. The BFGS algorithm requires an in-core storage of the vectors 𝒑𝑖 and 𝒒𝑖, 𝑖 = 1, … , 𝑘 − 1, and ∆𝒙𝑘−1 and 𝑭𝑘−1 to complete iteration 𝑘. It is the default and most robust quasi-Newton algorithm for the nonlinear implicit solver and there is no reason to switch. The only practical issue is how to control when to reform the tangent stiffness matrix, which typically depends on the degree of nonlinearity for the problem at hand. In fact, if LCPACK = 2 on CONTROL_IMPLICIT_SOLVER, i.e., working with independent variables only, BFGS is mandatory and comes in two flavors, NSOLVR = 2 or NSOLVR = 12 on CONTROL_IMPLICIT_SOLUTION. There is also the option LCPACK = 3, for which LS-DYNA uses a non-symmetric matrix assembly when solving the linear system of equations. This adds to the computational Implicit LS-DYNA Theory Manual cost for each iteration but my improve convergence because of better tangents of certain features. The non-symmetric solver is illustrated in Figure 3737-3 for simulating a clamped cantilever beam subject to a follower load. In general the stiffness matrix is symmetric when the force is derived from an energy potential, or in other words is conservative. This is for instance the case for a hyperelastic material response or a physically admissible pressure load, see Schweizerhof and Ramm [1984] for a discussion. Non-symmetry arise e.g. from non-conservative forces, such as frictional contact, or physically inadmissible design dependent loads. The example in Figure 3737-3 serves as one of the latter since the load is not coming from a physical source, such as a water pressure, and it should be seen as an academic example to prove a point. Follower load 𝐹 𝐹 = 1/16 𝐹 = 1/4 𝐹 = 1/2 𝐹 = 1 Figure 3737-3 Nonlinear implicit solution of an elastic cantilever beam with a follower force, von Mises stress is fringed.. 37.3.4 Tangent stiffness reformations In the previous section we have used 𝑲0 in (37.62) and (37.74) to represent the last assembled tangent stiffness matrix according to (37.33). While the quasi-Newton updates 𝑲𝑘, 𝑘 = 1,2, … are justified in the context of moderate nonlinearities and/or for a few iterations, it will eventually break down convergence for more complex problems. Whence there are criteria for reforming the tangent stiffness matrix and start over with the quasi-Newton (BFGS) updates. The first criterion is simply a user defined upper limit of 𝑘, governed by ILIMIT on CONTROL_IMPLICIT_SOLUTION. Using ILIMIT = 1 means that no quasi-Newton updates are performed and should be used for highly nonlinear problems, larger values LS-DYNA Theory Manual Implicit of ILIMIT can be used if the nonlinearities are considered less severe. ILIMIT = 11 is the default and is a reasonable value to use for starters. A second criterion is that of increased residual norm, i.e., if any of the quantities 𝑇𝑘 = ‖𝑱𝑡𝑭𝑘‖1 (37.75) or 𝑅𝑘 = ‖𝑱𝑟𝑭𝑘‖1 (37.76) for some 𝑘 is their respective largest attained since start iterating, the stiffness matrix is reformed. Here 𝑱𝑡 and 𝑱𝑟 are diagonal matrices with ones or zeros on the diagonal that extract the translational and rotational degrees of freedom, respectively, and one speaks of translational or rotational divergence. The notation ‖𝑭‖1 indicates the 𝐿1-norm of 𝑭, meaning the sum of the absolute value of its components. A third criterion is called energy explosion, if log(1 + ∣∆𝒙𝑘−1 𝑇 𝑱𝑡𝑭𝑘−1∣) + log(1 + ∣∆𝒙𝑘−1 𝑇 𝑱𝑡𝑭𝑘∣) > 36 (37.77) or log(1 + ∣∆𝒙𝑘−1 (37.78) the stiffness matrix is reformed. One can speak also here of translational and rotational energy explosion and this simply indicates that something really bad has happened with the last search direction. 𝑇 𝑱𝑟𝑭𝑘−1∣) + log(1 + ∣∆𝒙𝑘−1 𝑇 𝑱𝑟𝑭𝑘∣) > 36 Finally, a necessary criterion for continuing with BFGS updates is deemed ∆𝒙𝑘 (37.79) since this would otherwise indicate a search direction corresponding to a zero or negative eigenvalue in the tangent matrix. If this criterion is violated the tangent stiffness matrix is reformed with a warning message issued that negative energy is detected during quasi-Newton updates. This can only happen if there are negative eigenvalues in the tangent stiffness matrix in the first place. 𝑇𝑭𝑘 > 0 37.3.5 Line search Line search is critical for decent convergence characteristics, and there are several criteria to choose from, see LSMTD and LSTOL on CONTROL_IMPLICIT_SOLUTION. One of the criteria available is that the norm of residual 𝑭 must somehow decrease, LSMTD = 2, but this will inevitably lead to ridiculously small steps and is not recommended or presented further here. A more useful criterion is instead that an iterate 𝑘 + 1 is accepted if 𝑇𝑭𝑘 𝑇𝑭𝑘+1∣ ≤ 𝜀𝑠∆𝒙𝑘 ∣∆𝒙𝑘 (37.80) where 𝜀𝑠 is the line search convergence tolerance LSTOL. See Figure 3737-4 for an illustration. This criterion is derived from a hypothetical assumption of the existence of an energy potential 𝑊(𝒙𝑘 + 𝑠∆𝒙𝑘) for the residual force 𝑭 and that the potential is minimized along the search direction 𝜕𝑊 𝜕𝒙 = 𝑭 𝑇∆𝒙𝑘 = 0. 𝜕𝑊 𝜕𝑠 (37.81) 𝜕𝒙 𝜕𝑠 = Implicit LS-DYNA Theory Manual 𝑇∆𝒙𝑘 𝑭𝑘 𝑭 𝑇∆𝒙𝑘 (1.60) not solvable Acceptable interval according to (37.80) 𝜀𝑠𝑭𝑘 𝑇∆𝒙𝑘 𝑠 𝑠 = 1 Negative starting values indicate negative eigenvalues in tangent Figure 3737-4 Illustration of line search based on energy, may be complemented with norm of 𝑭. Dashed line indicates a line search that So in a sense, (37.80) is the solution of (37.81) to within a certain tolerance and a Ridder algorithm is used to narrowing in on a candidate. It is not unusual however that (37.80) is not well-posed, an indefinite stiffness matrix may result in a negative right hand side or the search direction may be bad enough to not render a solution, see Figure 3737-4. In those special cases some conservative approach is taken to provide a reasonable iterate 𝑘 + 1. This summarizes in brief LSMTD = 4. A closer examination (and numerical experiments) reveals that 𝑭𝑘+1 is not necessarily bounded by (37.80). Therefore this criterion can be complemented with ∥𝑭𝑘+1∥1 ≤ [1 + 𝜀𝑠]‖𝑭𝑘‖1. (37.82) where again ‖𝑭‖1 means the 𝐿1-norm of 𝑭. This option is invoked with LSMTD = 5 and means that both (37.80) and (37.82) are to be satisfied for accepting an iterate 𝑘 + 1. While this is a more robust approach, it also requires more residual force evaluations and is not recommended as default. It has proved to work well for implicit rubber simulations and complicated contact problems. 37.3.6 Convergence check Convergence criteria are based on displacement, energy and residual force quantities. The exact definitions of norms and scalar products used depend to a great extent on parameter settings on CONTROL_IMPLICIT_SOLUTION, in particular on the parameter NLNORM. Historically it has been assumed that rotational degrees of freedom are not appropriate for checking convergence and therefore only translational degrees of freedom have been considered. With advancements in the development of the implicit solver, this is today considered an old fashioned way of thinking, but backward compatibility is maintained and the user is referred to the keyword manual for information regarding the choices in this context. Here the principles behind LS-DYNA Theory Manual Implicit convergence checks are presented from a pragmatic standpoint assuming the following generic displacement and force norms and (energy) scalar products ‖∆𝒙‖ = √∆𝒙𝑇𝑱𝑱∆𝒙, ‖𝑭‖1 = ∑ ∣𝐽𝑖𝑖 †𝐹𝑖∣ , 〈∆𝒙, 𝑭〉 = ∆𝒙𝑇𝑱𝑱†𝑭. (37.83) Note that the norm of the incremenetal displacement is a 𝐿2-norm (euclidian norm) while the norm of the residual force is a 𝐿1-norm, this decision was made to allow for a more physical and less mesh dependent interpretation of this latter quantity. Here 𝑱 is a diagonal matrix that appropriately scales the various degrees of freedom to account for units, i.e., scaling radians with some characteristic length for consistency. It also accounts for user input in the sense that 𝑱 may contain zeros on the diagonal to indicate that rotational degrees of freedom should not be accounted for. 𝑱† is the pseudo-inverse of 𝑱, a notation introduced since 𝑱 actually may be singular due to the zeros on the diagonal. For some convergence option check is performed on translational and rotational degrees of freedom separately, we don’t elaborate on such details here but instead refer to the keyword manual. In (37.83), the non-bold quantities with subscripts indicate components of the corresponding bold-faced vector. Convergence for accepting an iterate 𝑗 + 1 is assumed if the three conditions ‖𝛥𝒙𝑘‖ < max(𝜀𝑑𝑢max, √max(𝜀𝑎, 0)) 〈∆𝒙𝑘, 𝑭𝑘〉 < max(𝜀𝑒𝑒0, 10000max(𝜀𝑎, 0)) ‖𝑭𝑘‖1 < max(𝜀𝑟𝑓0, 10000max(𝜀𝑎, 0)) (37.84 ) (37.85 ) (37.86) are satisfied simultaneously. Here 𝜀𝑑, 𝜀𝑒, 𝜀𝑟 and 𝜀𝑎 are the displacement, energy, residual and absolute tolerances corresponding to DCTOL, ECTOL, RCTOL and ABSTOL, respectively. In the right hand side of (37.84), 𝑢max = ∥𝒖max∥ is the maximum attained displacement in any iteration 𝑘 measured from the position at the start of this implicit step 𝑗 if DNORM = 1 and from the start of the simulation if DNORM = 2. In the right hand side of (37.85), 𝑒0 = 〈∆𝒙0, 𝑭0〉 where ∆𝒙0 and 𝑭0 are the first incremental displacement and residual vectors for this implicit step 𝑗. Likewise 𝑓0 = ∥𝑭0∥1 in the right hand side of (37.86) is the norm of the first residual vector for this implicit step 𝑗. If 𝑱 has full rank and the tangent stiffness matrix is symmetric and positive definite then these conditions make intuitive sense, small changes in displacements and/or small residual forces indicate that an iterate is “close-enough” to the solution. Under these conditions the left hand side of (37.85) define norms in both the incremental displacement ∆𝒙𝑘 and residual force 𝑭𝑘, and 𝑒0 > 0. Optionally, these convergence criteria can be combined with bounds on the maximum norms, here denoted ‖∆𝒙‖∞ = max|𝑱∆𝒙|𝑖, ‖𝑭‖∞ = max∣𝑱†𝑭∣ (37.87) where the max is taken over all nodes and rigid bodies in the model, i.e., 𝑖 ranges over all nodes and rigid bodies. If any of these options are activated, then convergence for 〈∆𝒙, 𝑭〉∞ = max∣∆𝒙𝑇𝑱𝑱†𝑭∣ , , Implicit LS-DYNA Theory Manual accepting an iterate 𝑗 + 1 is assumed if the three conditions (37.84), (37.85) and (37.86) are satisfied and ‖𝛥𝒙𝑘‖∞ < 𝜀𝑑 ∞𝑢max ∞ 〈∆𝒙𝑘, 𝑭𝑘〉∞ < 𝜀𝑒 ∞ ∞𝑒0 ‖𝑭𝑘‖∞ < 𝜀𝑟 ∞𝑓0 ∞ (37.88 ) (37.89 ) (37.90) ∞, 𝜀𝑒 ∞ and 𝜀𝑟 ∞ are the displacement, energy and residual tolerances are satisfied. Here 𝜀𝑑 corresponding to DMTOL, EMTOL and RMTOL, respectively, and if any of these parameters are zero that means the condition is not active. The remaining parameters on the right hand sides are interpreted in analogy to those appearing in the right hand sides of (37.84), (37.85) and (37.86), except for that the Euclidian norm is now substituted for the maximum norm. A backdoor out is an absolute convergence test on the maximum norm on translational displacement. That is, convergence is always detected if the maximum value of any translational degree of freedom in the incremental displacement array ∆𝒙𝑘 is smaller than 𝑑√max (𝜀𝑎, 0), where 𝑑 is a characteristic size calculated as the diagonal of the smallest box aligned along the global coordinate system that encapsulates the model. Setting ABSTOL to a negative number is an alternative, then all absolute convergence checks above become inactive and instead the backdoor out is to assume convergence when ‖𝑭𝑘‖1 < max(0, −𝜀𝑎). This latter option requires to some extent an a priori knowledge of the force level and may require monitoring the residual norm for a few trial iterations to pick a decent 𝜀𝑎, but it could be a sensible choice if the problem shows erratic behavior in displacement and energy due to severe nonlinearities. On the other hand, since it is a check on the 𝐿1-norm, the value 𝜀𝑎 might be taken as some reasonable fraction of an external load or as an desired error on the sum of inbalanced forces. Another criterion that must be met for convergence is that simple prescribed motion constraints on nodes and rigid bodies, if they exist, must be “almost” satisfied. The background is that only partial line searches (𝑠 < 1) will not satisfy simple motion constraints, and at least one full line search step (𝑠 = 1) must be accomplished during the iterations. For difficult problems, this sometimes never happens and therefore convergence is prevented due to unfulfilled boundary conditions until all prescribed motion is satisfied to within 1%. 37.3.7 Automatic time stepping If convergence is not attained after reforming the stiffness matrix a given amount of times, see MAXREF on CONTROL_IMPLICIT_SOLUTION, one of two things will happen. By default, LS-DYNA terminates with an error message, but if automatic time stepping is turned on, see IAUTO on CONTROL_IMPLICIT_AUTO, then LS-DYNA will try to resolve the problem with a smaller step size. More specifically, if LS-DYNA Theory Manual Implicit convergence is not attained with a time step ∆𝑡old, then LS-DYNA backs up to beginning of step and retries with a time step (37.91) where ∆𝑡min is a user defined minimum step. If ∆𝑡old = ∆𝑡min when attempting this then LS-DYNA will terminate with an error. ∆𝑡new = max(∆𝑡min, 10−0.3∆𝑡old) With the automatic time stepper turned on, LS-DYNA will not only cut the time step for convergence failure but also adjust the time step when converging. The adjustment is based on a user defined iteration window, i.e., a range of iteration numbers that are deemed acceptable for convergence, and if the number of iterations for convergence falls outside this window the next time step will be adjusted as follows. If convergence is attained for more iterations than acceptable then the time step for the next implicit step is given by (37.91). If instead convergence is attained for fewer iterations then the next time step is given by ∆𝑡new = min(∆𝑡max, 100.2∆𝑡old) (37.92) where ∆𝑡max is a maximum defined step. In this way LS-DYNA narrows in on an optimum time step for which the number of iterations to converge falls within the specified window. There is much more information regarding this option in the keyword manual and the user is referred thereto for practical issues. 37.4 Implicit Dynamics 37.4.1 Newmark time integration Nonlinear implicit dynamics principally follows the exact same solution algorithm as for nonlinear implicit statics, the only difference is that dynamic terms are included in the residual force. That is, (37.1) now reads (37.93) where global damping is introduced through the matrix 𝑫, so the residual is now essentially a function of 𝒙, 𝒙̇ and 𝒙̈. The dependence on the latter two is eliminated by introducing the Newmark time integration scheme 𝑹 = 𝑴𝒙̈ + 𝑫𝒙̇ + 𝑭𝑖 − 𝑭𝑒 = 𝟎, 𝒙̈ = 𝛥𝒙 𝛽𝛥𝑡2 − 𝒙̇𝑗 𝛽𝛥𝑡 − ( − 𝛽) 𝒙̈𝑗, 𝒙̇ = 𝒙̇𝑗 + 𝛥𝑡(1 − 𝛾)𝒙̈ 𝑗 + 𝛾𝛥𝑡𝒙̈, 𝒙 = 𝒙𝑗 + 𝛥𝒙. (37.94) (37.95) (37.96) Here, Δ𝑡 is the time step size, 𝛽 and 𝛾 are the free parameters of integration and we have used ∆𝒙 to denote the total displacement from step 𝑗 to step 𝑗 + 1. For 𝛾 = 1 ⁄ 2 and 𝛽 = 1 ⁄ 4 the method becomes the trapezoidal rule and is energy conserving. If Implicit LS-DYNA Theory Manual 𝛾 > , 𝛽 > ( + 𝛾) , (37.97) (37.98) numerical damping is induced into the solution leading to a loss of energy and momentum. By inserting (37.94) and (37.95) into (37.93) and using (37.96) to eliminate ∆𝒙, we are back to an equation in 𝒙 only and can apply the algorithm starting with (37.25) and everything thereafter holds. 37.4.2 Practical considerations Linearizing (37.93) using (37.94), (37.95) and (37.96) results in a tangent matrix 𝜕𝑹 𝜕𝒙 = 𝛽∆𝑡2 + 𝛾𝑫 𝛽∆𝑡 + 𝜕[𝑭𝑖 − 𝑭𝑒] 𝜕𝒙 , (37.99) and leads to an interesting observation. Since 𝑴 is symmetric and positive definite the first term assures that the resulting tangent is positive definite as long as the time step ∆𝑡 is sufficiently small, so including dynamics will enhance the robustness of the numerical procedure. In fact, the eigenvalues of the resulting tangent can be made arbitrarily large by decreasing ∆𝑡 at the cost of requiring more steps to obtain the solution. Not only robustness but also the accuracy in dynamic implicit depends on the size of the time step ∆𝑡, roughly speaking only frequencies up to ~∆𝑡−1 can be resolved. The method is therefore not perfectly suitable for contact-impact and restitution problems, for contact a crude rule of thumb is that the time a node or body is in contact should span at least a few time steps to appropriately resolve the resulting impulse. Having said this, these problems are still difficult to solve reasonably well. For implicit static contact problems, a common usage of dynamics is to temporarily suppress rigid body modes while a desired contact state is being established. In such a case it is recommended to use numerical damping by for instance choosing 𝛾 = 0.6 and 𝛽 = 0.38 to render a smooth response. This technique has proved successful and it is often sufficient to have dynamics initially turned on and then turned off at a time when all rigid body modes have been eliminated by contact. But it is also possible to arbitrarily switch dynamics on and off during a simulation, all this is explained on CONTROL_IMPLICIT_DYNAMICS in the keyword manual. 37.4.3 Linear theory Linearization of (37.93) with respect to a configuration 𝒙 that is in static equilibrium, i.e., 𝑷[𝑭𝑖 − 𝑭𝑒] = 𝟎, can be written as 𝑴𝒖̈ + 𝑫𝒖̇ + 𝑲𝒖 = 𝑭, (37.100) LS-DYNA Theory Manual Implicit where we use 𝒖 = ∆𝒙 to denote the displacement measured from the reference point 𝒙. For the sake of clarity we also abused some notation, using 𝑴 and 𝑫 to actually mean 𝑷𝑴𝑷𝑇 and 𝑷𝑫𝑷𝑇, respectively. Furthermore, 𝑲 denotes the sum of the material (37.39) and geometric (37.49) contributions to the static tangent stiffness matrix as well as any contributions from the external force, e.g., contacts, 𝑲 = 𝑷 ∫[𝑩𝑇𝑬𝑩 + 𝓑 𝑇𝝈𝓑]𝑑𝑉 𝑷𝑇 − 𝑷 𝜕𝑭𝑒 𝜕𝒙 𝑷𝑇. (37.101) The right hand side 𝑭 in (37.100) should be interpreted as an external (small) load that only depends on time 𝑡 and serves to dynamically perturb the static equilibrium. This equation can be discretized in time using the Newmark time integration scheme above and then efficiently integrated with no update of the tangent stiffness matrix between steps. This of course assumes that the displacements 𝒖 are small enough to not affect 𝑲 to great extent. Consider undamped free vibration in (37.100), i.e, 𝑫 = 𝟎 and 𝑭 = 𝟎, and transform this equation from time to frequency plane assuming constant 𝑴 and 𝑲. This results in an eigenvalue problem 𝑲𝒖 = 𝜔2𝑴𝒖 (37.102) that can be solved in LS-DYNA for the angular frequency 𝜔 and mode shape 𝒖. The stress 𝝈 in (37.101) affects the frequency 𝜔 in the following way. If the model is in a tensile state, i.e., the principal stresses are positive, then the eigenvalues of 𝑲 increase compared to a stress free state and from (37.102) the frequencies will increase. Conversely, the frequencies will decrease if the principal stresses decrease, this is the effect of tuning a guitar string by increasing or decreasing its tension. If linearizing with respect to a contact state, the last term in (37.101) will in effect constrain relative motion between parts or nodes in contact. More specifically, the relative normal displacement in 𝒖 will be zero, and the relative tangential motion will be governed by the present stick/slip condition. If in stick mode the relative tangential displacement in 𝒖 will be zero, and See CON- TROL_IMPLICIT_EIGENVALUE for the available options to solve (37.102). is unconstrained. in slip mode if it An example using modal analysis in this respect is shown in Figure 37.5. Implicit LS-DYNA Theory Manual 𝑓 = 15 𝐻𝑧 𝑓 = 40 𝐻𝑧 𝑓 = 43 𝐻𝑧 Figure 37.5. Intermittent eigenvalue analysis of tire. Model shown in top left, followed by lowest frequency modes for unpressurized tire (top right), inflated tire (bottom left) and inflated tire and frictional contact (bottom right). Resultant mode displacements are fringed. LS-DYNA Theory Manual Implicit In general 𝑫 ≠ 𝟎 and 𝑫 and/or 𝑲 may be non-symmetric as discussed in Section 37.3.3, but we assume 𝑴 is symmetric and positive definite and still 𝑭 = 𝟎. The characteristic equation approach for solving (37.100) makes use of the harmonic ansatz which is inserted into (37.100) to yield 𝒖(𝑡) = ∑ exp(𝜇𝑗𝑡)𝚽𝑗 ∑ exp (𝜇𝑗𝑡){𝜇𝑗 2𝑴 + 𝜇𝑗𝑫 + 𝑲}𝚽𝑗 = 𝟎 (37.103) (37.104) to which the quadratic eigenvalue problem is associated7 {𝜇2𝑴 + 𝜇𝑫 + 𝑲}𝚽 = 𝟎. (37.105) Because of the non-symmetry of the involved matrices, the eigenvalues to (37.105) may be complex but come in conjugate pairs. That is, if 𝜇 = 𝑟 + 𝑖𝑠 is an eigenvalue then 𝜇̅̅̅̅ = 𝑟 − 𝑖𝑠 is also an eigenvalue, and if 𝚽 = 𝚼 + 𝑖𝚿 is the eigenvector associated with 𝜇 then 𝚽̅̅̅̅̅̅ = 𝚼 − 𝑖𝚿 is the eigenvector for 𝜇̅̅̅̅. However, examining the sum of two such terms in (37.104) yields exp(𝜇𝑡){𝜇2𝑴 + 𝜇𝑫 + 𝑲}𝚽 + exp(𝜇̅̅̅̅𝑡){𝜇̅̅̅̅2𝑴 + 𝜇̅̅̅̅𝑫 + 𝑲}𝚽̅̅̅̅̅̅ = 2exp(𝑟𝑡){((𝑟2 − 𝑠2)𝑴 + 𝑟𝑫 + 𝑲)(cos(𝑠𝑡) 𝚼 − 𝑠𝑖𝑛(𝑠𝑡)𝚿) (37.106) − 𝑠(2𝑟𝑴 + 𝑫)(sin(𝑠𝑡) 𝚼 + cos(𝑠𝑡)𝚿)}, meaning that the solution in time domain is real as expected. If all eigenvalues are purely complex, i.e., 𝜇𝑗 = 𝑖𝑠𝑗 and the real parts 𝑟𝑗 = 0 vanish, then the solution to (37.100) is harmonic with angular frequencies 𝜔𝑗 = ∣𝑠𝑗∣. This is apparent from (37.106) and corresponds to the traditional solution to (37.102), with the exception of a non-zero damping matrix 𝑫. But if an eigenvalue has a real part 𝑟𝑗 > 0 then from (37.106) the solution is exponentially growing and thus unstable. Solving (37.105) can therefore be used to detect instabilities in a system, eigenvalues with positive real parts correspond to unstable modes. A common indicator used for this is the damp ratio defined as 𝜗 = −2 |𝑠| so basically a negative damp ratio indicates an unstable mode. An application of this is brake squeal, see Figure 37.6, for which friction instabilities may result in unwanted noise and erratic behavior. Noticable is that if 𝑫 = 𝟎 and 𝜇 is an eigenvalue then – 𝜇 is also an eigenvalue, so then complex eigenvalues come in clusters of four, {𝜇, 𝜇̅̅̅̅, −𝜇, −𝜇̅̅̅̅}. Then it suffice that eigenvalues have nonzero real parts 𝑟𝑗 ≠ 0 for a system to be unstable, which corresponds to negative eigenvalues in (37.102). To solve the system (37.105), it is transformed to a first order eigenvalue problem using 𝚽̃ = 𝜇𝚽, resulting in , (37.107) [ 𝟎 −𝑲 −𝑫 ][𝚽 𝚽̃] = 𝜇[𝑰 𝟎 𝑴 ][𝚽 𝚽̃], (37.108) which can be solved by well-established eigenvalue algorithms. In the output files, LS- DYNA reports eigenvalues with positive imaginary parts only, i.e., 𝑠𝑗 > 0, and the real and imaginary parts (when non-zero) of the associated eigenvector 𝚽. 7 The eigenvalue problem (1.105) is readily obtained by Laplace transforming (1.100). Implicit LS-DYNA Theory Manual 0.02 0.015 0.01 0.005 0 -0.005 -0.01 -0.015 -0.02 0 2 4 6 8 10 12 14 16 Mode Figure 37.6. Brake squeal application. Pressure pads are applied to a rotating disc and a nonsymmetric eigenvalue solution reveals friction instabilities. The damp ratio 𝜗 is plotted at the top as function of mode number, see (37.107). Mode #6 is the unstable mode and is depicted bottom right with displacements fringed. LS-DYNA Theory Manual Arc-length 38 Arc-length Arc-length methods are available in LS-DYNA for NSOLVR specified between 6 and 9, this and all other parameters in this Section are located on the *CONTROL_IMPLICIT_- SOLUTION keyword. These solvers use the Riks/Crisfield methods but unfortunately go under the old LSDIR.EQ.1 option which makes them somewhat limited in terms of applicability. For LSDIR.EQ.2 the arc-length method described in Ritto-Corrêa and Camotim [2008] implemented for the combination of NSOLVR.EQ.12 and ARCMTH.EQ.3. For this method the parameters ARCPSI (𝜓), ARCALF (𝛼) and ARCTIM apply, out of which the last simply tells at what time arc-length is initiated and the first two are to be described in more detail below. We begin by an explanatory overview of the arc-length method in general for which we will constantly be referring to Figure 38.1 below. After that the mathematical details are revealed. is 38.1 Overview An implicit static problem is driven by a parameter 𝑡 referred to as the time, and assuming that a solution is obtained at 𝑡 = 𝑡𝑛 the objective is to determine the solution given the constraint 𝑡 = 𝑡𝑛+1, where 𝑡𝑛+1 is given. We assume that the problem can be associated with representative force and displacement parameters 𝑓 and 𝑑 and we distinguish between load- and displacement-driven problems. An example of a load- driven problem is when 𝑓 = 𝑓 (𝑡) is an external load and 𝑑 is the resulting displacement of the associated nodes, and likewise a displacement-driven problem is when 𝑑 = 𝑑(𝑡) is a prescribed displacement and 𝑓 is the corresponding reaction force. A solution is likely obtained if the problem is stable, i.e., the force-displacement curve is monotonically increasing, but this method is not designed to handle limit or turning points. A limit point is illustrated in figure (a) and a turning point in figure (b), the solution in the next step may not be the one desired or not even exist, in both cases we want to find the solution that continuously follow the path corresponding to the force-displacement curve. Arc-length LS-DYNA Theory Manual The solution for this is to set the stepping parameter 𝑡 free, i.e., replace the constraint 𝑡 = 𝑡𝑛+1 with an arc-length constraint 𝑔(𝑑, 𝑓 ) = 0. In words, this basically means that a multidimensional sphere (arc) is put around the last converged solution and the next solution is to be found on that given sphere, the stepping parameter 𝑡 is now a solution variable. This makes the problem well-posed but unfortunately there are multiple solutions to the problem, and it may turn out that the wrong solution is found. In figures (c) and (d), the effect of the arc-length constraints is illustrated and there are two possible solutions, one feasible that allows us to continue in the right direction and one infeasible that takes us in the wrong direction. The latter phenomenon is termed doubling back, and is in practice not easily avoided. Two additional parameters are available that have shown to improve the robustness in this respect. LS-DYNA Theory Manual Arc-length a) b) c) e) g) d) f) ff h) Converged solution at step n Infeasible solution at step n + 1 Feasible solution at step n + 1 Center of arc for α < 0, makes infeasible solution less probable Figure 38.1. Representative force-displacement curves for illustrating arc- length and accompanying parameters In figure (d), two of the infeasible solutions can in practice be avoided by including the stepping parameter in the arc-length constraint, thus converting a cylinder to a sphere in space-time. This is adjusted by the paremeter 0 ≤ 𝜓 < 1, and the constraint reads (1 − 𝜓)𝑔(𝑑, 𝑓 ) + 𝜓(𝑡 − 𝑡𝑛)2 = 0, the effect of this constraint is illustrated in figures (e) and (f), and should be compared with figures (c) and (d). Note that two infeasible solutions are avoided when comparing figures (d) and (f), it may sometimes be worth using a non-zero value for 𝜓, e.g., 𝜓 = 0.1. Arc-length LS-DYNA Theory Manual Another problem is that the feasible and infeasible solution may be too close to the last converged solution, making the result from the simulation very unpredictable. For this a parameter 𝛼 is introduced that translates the center of the spatial sphere in the direction of the linear prediction (i.e., the first Newton iterate of the implicit solution procedure). Assuming that this prediction is in the direction we want, using 𝛼 < 0 will move the center, and consequently the infeasible solution, away from where the iterates are taking place. In addition, the radius of the arc will increase making it less probable to find the incorrect solution. This option has shown effective in solving snap-through problems when using small steps to resolve maximum load values, and is illustrated in figures (g) and (h). For snap-back problems, using 𝛼 = 1 could be an interesting choice since this centers the arc right between the previously converged point and the first predictor in the arc length method, thus encouraging the next solution to be found in the reversed direction. An example of a snap-back problem is shown in Figure 38-3. 38.2 Nonlinear equations The following, except for a change in notation, is very similar to the nonlinear theory presented in the previous chapter. The generalization is that 𝑡 will here be treated as an independent variable that is constrained by arc-length instead of given as a constant. The nonlinear variables are denoted 𝒙 = [ 𝒙𝐼 𝒙𝐷 ], (38.1) that we assume can be divided into a set of independent and dependent variables. Furthermore we have the time parameter 𝑡 which may serve as the actual time (for dynamic problems) or just a stepping parameter (for quasi-static problems). The division into independent and dependent variables is motivated by the constraint equation that must be fulfilled, i.e., From the constraint, the constraint matrix is evaluated as 𝒉(𝒙, 𝑡) = 𝒉(𝒙𝐼, 𝒙𝐷, 𝑡) = 𝟎. 𝜕𝒉 𝜕𝒙 = [ 𝜕𝒉 𝜕𝒙𝐼 𝜕𝒉 𝜕𝒙𝐷 ] = [𝑪𝐷𝐼 𝑪𝐷𝐷], (38.2) (38.3) which in turn determines the space of trial functions used to establish the nonlinear finite element equation, [𝑰𝐼𝐼 −(𝑪𝐷𝐷 −1 𝑪𝐷𝐼) 𝑇][ 𝒓𝐼 𝒓𝐷 ] = 𝟎, where 𝒓(𝒙, 𝑡) = 𝒓(𝒙𝐼, 𝒙𝐷, 𝑡) = [ 𝒓𝐼 𝒓𝐷 ] (38.4) (38.5) is the full residual divided into the set of independent and dependent variables. See previous chapter for further details leading up to (38.4). LS-DYNA Theory Manual Arc-length 38.3 Newton iterations Here we assume that we are in a given configuration given by 𝒙(𝑛,𝑖) = 𝒙(𝑛) + ∆𝒙(𝑛,𝑖), 𝑡(𝑛,𝑖) = 𝑡(𝑛) + ∆𝑡(𝑛,𝑖). (38.6) where superscript 𝑛 = 0, 1, 2, … represents converged implicit states and 𝑖 = 0, 1, 2, … represents non-converged Newton iterates. We implicitly assume that 𝒙(0) = 𝒙̅, ∆𝒙(𝑛,0) = 𝟎, 𝑡(0) = 0 and ∆𝑡(𝑛,0) = 0 are given. In this configuration LS-DYNA computes the full residual given as as well as its dependence on the time parameter 𝒓(𝑛,𝑖) = [ 𝒓𝐼 𝒓𝐷 ], (𝑛,𝑖) ) = ( 𝜕𝒓 𝜕𝑡 𝜕𝒓𝐼 ⎤ ⎡ 𝜕𝑡 ⎥⎥⎥ ⎢⎢⎢ , 𝜕𝒓𝐷 𝜕𝑡 ⎦ ⎣ together with the stiffness matrix given as (𝑛,𝑖) ) = [ ( 𝜕𝒓 𝜕𝒙 𝑲𝐼𝐼 𝑲𝐼𝐷 𝑲𝐷𝐼 𝑲𝐷𝐷 ]. (38.7) (38.8) (38.9) Likewise the constraint residual, its dependence on the time parameter and constraint matrix are evaluated and given by 𝒉(𝑛,𝑖) = 𝒉, (𝑛,𝑖) 𝜕𝒉 𝜕𝑡 , ) = (𝑛,𝑖) ( ( 𝜕𝒉 𝜕𝑡 𝜕𝒉 𝜕𝒙 ) = [𝑪𝐷𝐼 𝑪𝐷𝐷]. The reduced residual and stiffness matrix are then formed as 𝑲̂𝐼𝐼 = [𝑰𝐼𝐼 −(𝑪𝐷𝐷 −1 𝑪𝐷𝐼) 𝑇] [ 𝒓 ̂𝐼 = [𝑰𝐼𝐼 −(𝑪𝐷𝐷 −1 𝑪𝐷𝐼) 𝑇] {[ 𝜕𝒓 ̂𝐼 𝜕𝑡 = [𝑰𝐼𝐼 −(𝑪𝐷𝐷 −1 𝑪𝐷𝐼) 𝑇] ] − [ 𝑲𝐼𝐼 𝑲𝐼𝐷 𝑲𝐷𝐼 𝑲𝐷𝐷 𝒓𝐼 𝑲𝐼𝐷 𝒓𝐷 𝑲𝐷𝐷 ⎧ {{ ⎨ {{ ⎩ 𝜕𝒓𝐼 ⎤ ⎡ 𝜕𝑡 ⎥⎥⎥ ⎢⎢⎢ 𝜕𝒓𝐷 𝜕𝑡 ⎦ ⎣ − [ ] [ 𝑰𝐼𝐼 −1 𝑪𝐷𝐼 −𝑪𝐷𝐷 −1 𝒉} , ] 𝑪𝐷𝐷 ] , 𝑲𝐼𝐷 𝑲𝐷𝐷 ] 𝑪𝐷𝐷 −1 𝜕𝒉 𝜕𝑡 ⎫ }} ⎬ }} ⎭ , (38.10) (38.11) and the independent search direction is given by 𝛿𝒙𝐼 = 𝑠𝛿𝒙𝐼 𝑠 + 𝛿𝑡 𝜕𝒙𝐼 𝜕𝑡 . LS-DYNA Draft Arc-length LS-DYNA Theory Manual Here 𝑠 is the line search parameter and 𝑠 = −𝑲̂𝐼𝐼 𝛿𝒙𝐼 𝜕𝒙𝐼 = −𝑲̂𝐼𝐼 𝜕𝑡 −1𝒓 ̂𝐼, −1 𝜕𝒓 ̂𝐼 𝜕𝑡 . The full search direction is completed by computing the dependent part as 𝛿𝒙𝐷 = 𝑠𝛿𝒙𝐷 𝑠 + 𝛿𝑡 𝜕𝒙𝐷 𝜕𝑡 , where 𝑠 = −𝑪𝐷𝐷 𝛿𝒙𝐷 𝜕𝒙𝐷 𝜕𝑡 Finally the new configuration is updated by means of 𝑠 − 𝑪𝐷𝐷 −1 𝑪𝐷𝐼𝛿𝒙𝐼 𝜕𝒙𝐼 −1 𝑪𝐷𝐼 𝜕𝑡 −1 𝒉, −1 𝜕𝒉 𝜕𝑡 = −𝑪𝐷𝐷 − 𝑪𝐷𝐷 . (𝑛,𝑖+1) = ∆𝒙𝐼 (𝑛,𝑖+1) = ∆𝒙𝐷 ∆𝒙𝐼 ∆𝒙𝐷 ∆𝑡(𝑛,𝑖+1) = ∆𝑡(𝑛,𝑖) + 𝛿𝑡. (𝑛,𝑖) + 𝛿𝒙𝐼, (𝑛,𝑖) + 𝛿𝒙𝐷, Upon convergence we set and hence (𝑛,𝑖+1), (𝑛) = ∆𝒙𝐼 ∆𝒙𝐼 (𝑛,𝑖+1), (𝑛) = ∆𝒙𝐷 ∆𝒙𝐷 ∆𝑡(𝑛) = ∆𝑡(𝑛,𝑖+1), (𝑛) + ∆𝒙𝐼 (𝑛+1) = 𝒙𝐼 𝒙𝐼 (𝑛) + ∆𝒙𝐷 (𝑛+1) = 𝒙𝐷 𝒙𝐷 𝑡(𝑛+1) = 𝑡(𝑛) + ∆𝑡(𝑛). (𝑛) , (𝑛), (38.13) (38.14) (38.15) (38.16) (38.17) (38.18) LS-DYNA Theory Manual Arc-length Previously converged solution Infeasible solution Feasible solution Predictore solution, found in the outward Normal direction of previous arc Infeasible predictor solution Corrector steps occur along the arc Figure 38.2. Predictor and corrector steps 38.4 Arc-length constraint – predictor step For the predictor step, 𝑖 = 0, the following constraint is imposed (1 − 𝜓) (𝑛,1)) (∆𝒙𝐼 (0,1)) (∆𝒙𝐼 (𝑛,1) ∆𝒙𝐼 (0,1) ∆𝒙𝐼 + 𝜓 ∆𝑡(𝑛,1)∆𝑡(𝑛,1) ∆𝑡(0,1)∆𝑡(0,1) − 1 = 0, where for 𝑛 = 0 we use (0,1) = ∆𝑡 ̅ ∆𝒙𝐼 ∆𝑡(0,1) = ∆𝑡 ̅. 𝜕𝒙𝐼 𝜕𝑡 (38.19) (38.20) Arc-length LS-DYNA Theory Manual Referring to Figure 38.2 this constraint is geometrically interpreted as to find a predictor solution on the arc with the previously converged solution as its center. Writing out the above in terms of known quantities results in the following two possible values of the increment in time step parameter 𝛿𝑡± = ± 𝜕𝒙𝐼 𝜕𝑡 𝑇 𝜕𝒙𝐼 𝜕𝑡 ) ⎜⎛𝜓𝑥 ( ⎝ + 𝜓𝑡 ⎟⎞ ⎠ −1/2 , corresponding to the two possible predictor solutions on the arc, where 𝜓𝑥 = 𝜓𝑡 = , 1 − 𝜓 (0,1)) ∆𝒙𝐼 (∆𝒙𝐼 ∆𝑡(0,1)∆𝑡(0,1). (0,1) (38.21) (38.22) The actual value used is detemined from the sign of 𝑇 𝜕𝒙𝐼 𝜕𝑡 (𝑛−1,1)) (𝑛−1) − 2 (∆𝒙𝐼 ∆𝒙𝐼 𝜓𝑥 (1 − 𝛼 ) + 𝜓𝑡∆𝑡(𝑛−1), (38.23) if positive 𝛿𝑡 = 𝛿𝑡+, otherwise 𝛿𝑡 = 𝛿𝑡−. This condition is to say that the solution continues in the direction of the previously converged state, for the initial step 𝑛 = 0, 𝛿𝑡 = 𝛿𝑡+. Again referring to Figure 38.2 we simply want to avoid going backwards to the infeasible predictor solution. 38.5 Arc-length constraint – corrector steps For the corrector steps, 𝑖 > 0, the following constraint is imposed (1 − 𝜓) (∆𝒙𝐼 (𝑛,𝑖+1) − 𝛼 ∆𝒙𝐼 (1 − 𝛼 ) (𝑛,1)) (∆𝒙𝐼 (0,1)) (𝑛,𝑖+1) − 𝛼 (0,1) ∆𝒙𝐼 (∆𝒙𝐼 (𝑛,1)) ∆𝒙𝐼 + 𝜓 ∆𝑡(𝑛,𝑖+1)∆𝑡(𝑛,𝑖+1) ∆𝑡(0,1)∆𝑡(0,1) − 1 = 0, (38.24) which geometrically says that we should find the next iterate on the arc. Expanding, this amounts to (𝑛,𝑖) + 𝑠𝛿𝒙𝐼 𝛼𝑥 (∆𝒙𝐼 𝛼𝑡(∆𝑡(𝑛,𝑖) + 𝛿𝑡)(∆𝑡(𝑛,𝑖) + 𝛿𝑡) − 1 = 0, 𝑠 + 𝛿𝑡 ∆𝒙𝐼 − (𝑛,1)) 𝜕𝒙𝐼 𝜕𝑡 (∆𝒙𝐼 (𝑛,𝑖) + 𝑠𝛿𝒙𝐼 𝑠 + 𝛿𝑡 𝜕𝒙𝐼 𝜕𝑡 − (𝑛,1)) + ∆𝒙𝐼 (38.25) where 𝛼𝑥 = 𝛼𝑡 = 1 − 𝜓 (0,1)) ) (1 − 𝛼 (∆𝒙𝐼 ∆𝑡(0,1)∆𝑡(0,1). (0,1) ∆𝒙𝐼 (38.26) LS-DYNA Theory Manual Arc-length This can be written in terms of a polynomial in 𝑠 and 𝛿𝑡 as 𝑎𝑠𝑠𝑠2 + 𝑎𝑡𝑡𝛿𝑡2 + 2𝑎𝑠𝑡𝑠𝛿𝑡 + 2𝑎𝑠𝑠 + 2𝑎𝑡𝛿𝑡 where + 𝛼𝑡 ) 𝑎𝑡𝑡 = 𝛼𝑥 ( 𝑠)𝑇𝛿𝒙𝐼 𝑎𝑠𝑠 = 𝛼𝑥 (𝛿𝒙𝐼 𝑇 𝜕𝒙𝐼 𝜕𝒙𝐼 𝜕𝑡 𝜕𝑡 𝑠)𝑇 𝜕𝒙𝐼 𝜕𝑡 𝑠)𝑇 𝜕𝒙𝐼 𝜕𝑡 (𝑛,𝑖) − 𝑎𝑠𝑡 = 𝛼𝑥(𝛿𝒙𝐼 𝑎𝑠𝑡 = 𝛼𝑥(𝛿𝒙𝐼 𝑎𝑠 = 𝛼𝑥 (∆𝒙𝐼 𝑎𝑡 = 𝛼𝑥 (∆𝒙𝐼 (𝑛,𝑖) − (𝑛,1)) ∆𝒙𝐼 + 𝛼𝑡∆𝑡(𝑛,𝑖). (𝑛,1)) ∆𝒙𝐼 𝑠 𝛿𝒙𝐼 𝑇 𝜕𝒙𝐼 𝜕𝑡 (38.27) (38.28) For a given line search parameter value, the time increment can have two possible values 𝛿𝑡± = −𝑎𝑠𝑡𝑠 − 𝑎𝑡 ± √(𝑎𝑠𝑡 2 − 𝑎𝑡𝑡𝑎𝑠𝑠)𝑠2 + 2(𝑎𝑠𝑡𝑎𝑡 − 𝑎𝑠𝑎𝑡𝑡)𝑠 + 𝑎𝑡 . (38.29) 𝑎𝑡𝑡 and the value we use for the update is given by 𝛿𝑡 = 𝛿𝑡+ if 𝑎𝑡 ≥ 0, otherwise 𝛿𝑡 = 𝛿𝑡−. This decision is based on the requirement of having 𝛿𝑡 → 0 when 𝑠 → 0. Arc-length LS-DYNA Theory Manual Panel Response 1 0.8 0.6 0.4 0.2 0 0 0.2 0.4 0.6 0.8 1 1.2 1.4 Displacement Figure 38-3 Snap-back buckling of panel, normalized force displacement curve shown LS-DYNA Theory Manual Sparse Direct Linear Equation Solvers 39 Sparse Direct Linear Equation Solvers LS-DYNA has 5 options for direct solution of the sparse systems of linear equations that arise in LS-DYNA. All 5 options are based on the multifrontal algorithm [Duff and Reid, 1983]. Multifrontal is a member of the current generation of sparsity preserving factorization algorithms that also have very fast computational rates. That is multifrontal works with a sparsity preserving ordering to reduce the overall size of the direct factorization and the amount of work it takes to compute that factorization. 39.1 Sparsity Preserving Orderings In LS-DYNA there are two ordering algorithms for preserving the sparsity of the direct factorization. The algorithms are Multiple Minimum Degree (MMD) and METIS [Karypis and Kumar, 1998]. MMD computes the ordering using locally based decisions and a bottom-up approach. It is inexpensive and very effective for small problems that are problems with fewer than 100,000 rows. METIS computes the ordering from a top down approach. While METIS usually takes more time than MMD to compute the ordering, the METIS ordering reduces the work for the factorization enough to recover the additional ordering cost. METIS is especially effective for large problems, especially those that are modeling three-dimensional solids. The user can specify either algorithm using keyword *CONTROL_IMPLICIT_- LINEAR. The default is to use MMD for problems with fewer than 100,000 rows and METIS for problems with more than 100,000 rows. We recommend that the user try both orderings as sometimes MMD is better than METIS on large problems that are not three-dimensional solids. Sparse Direct Linear Equation Solvers LS-DYNA Theory Manual 39.2 Multifrontal Algorithm The multifrontal algorithm factors a sparse matrix in a way that vastly reduces the amount of work required to compute the factorization compared to methods such as the frontal, profile, skyline, and variable band. These older methods counted on clustering the nonzero entries of the factorization close to the diagonal to keep the size of the factorization and the amount of work required to compute the factorization to a minimum. The factorization was then computed in a serial, left-to-right fashion, essentially following a chain of computations. The multifrontal algorithm instead follows a tree of computations where the tree structure is established by the sparsity preserving orderings, See Figure 39.1. It is this tree structure that greatly reduces the work required to compute a factorization and the size of the resulting factorization. At the bottom of the tree, a frontal matrix is assembled with the original matrix data and those columns that are fully assembled are eliminated. The remainder of the frontal matrix is updated from the factored columns and passed up the tree to the parent front in what is called an update matrix. As the computation works its way up the tree, a frontal matrix is formed by assembling the original matrix data and the update matrices from its children in the tree. The fully assembled columns are factored and the remaining columns updated and passed up the tree. At the root (top) of the tree, the remaining columns are factored. By organizing the factorization as a sequence of partial factorization of dense frontal matrices, the multifrontal algorithm can be very fast in performing the required computations. It can use all of the modern technology for dense linear algebra to get high performance computational kernels that should achieve near peak computational performance for a given processor. Only 1% to 5% of the work of the factorization is performed with slower operations such as scatter/gather. LS-DYNA Theory Manual Sparse Direct Linear Equation Solvers original matrix data From children fronts To parent front computations in single front Figure 39.2. Single front algorithm. 39.3 The Five Solver Options In LS-DYNA three new direct solution options were added. For backward compatibility, the two older options were kept. The five options are: Multifrontal elimination tree Figure 39.1. Multifrontal algorithm. Solver Method Sparse Direct Linear Equation Solvers LS-DYNA Theory Manual No. 1 3 4 5 6 Older implementaion of Solver No. 4. Uses Real*4 arithmetic, has out of memory capabilities as well as distributed memory parallelism. Only uses MMD ordering. Was former default method. Retained for backward compatibility. We recommend switching to Solver No. 4 for improved performance. Same as 1 except uses Real*8 arithmetic. We recommend switching to Solver No. 5 or 6 for improved performance. Real*4 implementation of multifrontal which includes automatic out-of- memory capabilities as well as distributed memory parallelism. Can use either MMD or METIS orderings. Default method. Real*8 implementation of Solver No. 4. Multifrontal solver from BCSLIB-EXT [Boeing Company, 1999]. Uses Real*8 arithmetic with extensive capabilities for large problems and some Shared Memory Parallelism. Can use either MMD or METIS orderings. If the other solvers cannot factor the problem in the allocated memory, try using this solver. We strongly recommend using Solvers 4 through 6. Solvers 1 and 3 are included for backward compatibility with older versions of LS-DYNA but are slower the Solvers 4 through 6. Solvers 4 and 5 are 2 to 6 times faster than the older versions, respectively. Solver 6 on a single processor computer should be comparable to Solver 5 but has more extensive capabilities for solving very large problems with limited memory. Solvers 4 and 5 should be used for distributed memory parallel implementations of LS-DYNA. Solver 6 can be used in shared memory parallel. In an installation of LS-DYNA where both integer and real numbers are stored in 8 byte quantities, then Solvers 1 and 3 are equivalent and Solvers 4 and 5 are equivalent. 39.4 Treating Matrix Singularities LS-DYNA has two different techniques for preventing singularities in the stiffness matrix, K. The most common type of matrix singularity arises from the use of certain types of shell elements. These shell elements generate no matrix contribution in the normal direction for each node. Depending on the geometry around the node and what other types of elements are connected to the node, there may or may not be a matrix singularity associated with the rotation around the normal direction at one or more nodes. This is commonly called the drilling rotation singularity. The first way LS-DYNA has for preventing such matrix singularities is to add a small amount of stiffness in the normal direction at each node of every shell element that has the drilling rotation problem. This “drilling” stiffness matrix is orthogonal to LS-DYNA Theory Manual Sparse Direct Linear Equation Solvers rigid body motions. The user can control whether this approach is used and how much stiffness is added via the *CONTROL_IMPLICIT_SOLUTION keyword card. DRLMTH and DRLPARM are set in fields 5 and 6. If DRLMTH = 1 then this approach is used. The amount of stiffness added is controlled via DRLPARM. The default for DRLPARM is 1.0 for linear problems and 100.0 for nonlinear problems. DRLPARM ∗ .0001 is added in the normal direction at each node to the diagonal terms associated with the rotational degrees of freedom for certain types of elemental matrices. For eigenvalue problems the amount of stiffness added is 1.E-12. Adding stiffness to handle the drilling rotation problem has been used extensively. While a robust and reliable approach, its drawback is that the added stiffness may affect the quality of the computed results. The user can also select not to use this approach and depend solely on AUTOSPC, the other method for preventing matrix singularities. AUTOSPC stands for AUTOmatic Single Point Constraints. AUTOSPC examines K after all of the elemental matrices have been assembled and all of the constraints have been applied for columns that are singular. The user controls AU- TOSPC using ASPCMTH and ASPCTOL, fields 7 and 8 of the CONTROL_IMPLICIT_- SOLUTION keyword card. If ASPCMTH = 1, AUTOSPC is used. For every set of columns of K that correspond to the translational or rotational degrees of freedom for a node or rigid body those columns are examined. The singular values of the diagonal block of the columns are computed. If the ratio of the smallest and largest singular values is less than ASPCTOL then the set of the columns is declared singular and a constraint is imposed to remove the singularity. The defaults for ASPCTOL is 1.E-6 when the matrix is assembled in REAL*4 precision and 1.E-8 when REAL*8 is used. The imposed constraint sets the degree of freedom to zero that is associated with the column that has the largest component in the null space of the columns. If all of the singular values are less than ASPCTOL all of the degrees of freedom in the block are constrained to zero. LS-DYNA Theory Manual Sparse Eigensolver 40 Sparse Eigensolver LS-DYNA now includes the Block Shift and Invert Lanczos eigensolver from BCSLIB-EXT. This eigensolver is used in LS-DYNA to compute the normal modes and mode shapes for the vibration analysis problem where 𝐊 and 𝐌are the assembled stiffness and mass matrices, 𝚽 are the eigenvectors (normal mode shapes) and 𝚲 are the eigenvalues (normal modes). 𝐊𝚽 = 𝐌𝚽𝚲, (40.1) The Lanczos algorithm iteratively computes a better and better approximation to the extreme eigenvalues and the corresponding eigenvectors of the ordinary eigenvalue problem 𝐀𝚽 = 𝚽𝚲where 𝐀 is a real symmetric matrix using only matrix-vector multiplies. To use Lanczos on the vibration analysis problem it must be changed to (𝐊 − 𝛔𝐌)−1𝐌𝚽 = 𝚽𝚯, (40.2) where each shifted and inverted eigenvalue 𝜃𝑖 = 1/(𝜆𝑖 − 𝜎). This change to an ordinary eigenvalue problem makes the eigenvalues of the original problem near σ become the extreme eigenvalues of the ordinary eigenvalue problem. This helps the Lanczos algorithm compute those eigenvalues quickly. BCSLIB-EXT uses a sophisticated logic to choose a sequence of shifts, 𝜎𝑖, to enable the computation of a large number of eigenvalues and eigenvectors. At each shift the factorization of 𝐊 − 𝛔𝐌 is computed. The factorization provides the matrix inertia that tells the algorithm how many eigenvalues are to the left of any given 𝜎𝑖. Given the inertia information, BCSLIB-EXT can tell how many eigenvalues are in a given interval and determine if all of the eigenvalues in that interval have been computed. As a result, BCSLIB-EXT is a very robust eigensolver. The implementation of BCSLIB-EXT in LS-DYNA includes a shared memory implementation. However only limited parallel speed-up is available for most problems. This is because the eigensolution requires a vast amount of data that for most problems this data has to be stored on I/O files. The wall clock time for the Sparse Eigensolver LS-DYNA Theory Manual eigensolver is as much a function of the speed of the I/O subsystem on the computer as the CPU time. Parallelism can only speed up the CPU time and does nothing to speed- up the I/O time. The user can request how many and which eigenvalues to compute using the keyword *CONTROL_IMPLICIT_EIGENVALUE. Via the parameters on this keyword, the user can request any of the following problems: • Compute the lowest 50 modes (that is nearest to zero) • Compute the 20 modes nearest to 30 Hz. • Compute the lowest 20 modes between 10 Hz and 50 Hz. • Compute all of the modes between 10 Hz and 50 Hz. • Compute all of the modes below 50 Hz. • Compute the 30 modes nearest to 30 Hz between 10 Hz and 50 Hz. 40.1 The Eigenvalue Problem for Rotating Systems Rotating systems, such as the compressor and turbine assembly of a jet engine, have large inertial forces that are functions of the distance from the axis of rotation. These forces are naturally generated in LS-DYNA if the system is modeled as rotating at the proper angular velocity. However, this is often inconvenient for postprocessing because the solution has an oscillatory character imposed it due to the rotation. A commonly used approach to bypass this difficulty is to impose body forces that are equivalent to the inertial forces due to rotation. In LS-DYNA, these forces are imposed through *LOAD_BODY_GENERALIZED and related keywords. For a system with a constant angular velocity 𝛚 = {𝜔𝑥, 𝜔𝑦, 𝜔𝑧}T, the body force added to the applied load is 𝐅B = −𝐌{2𝛚 × 𝐮̇ + 𝛚 × (𝛚 × (𝐫 + 𝐮))}. (40.3) In this equation, 𝐫 is the initial coordinate at a point and 𝐮 is the displacement. Because the body force is a function of both the velocity and displacement, it contributes both damping and stiffness matrices to the eigenvalue problem. Furthermore, since the term involving the initial coordinate creates an initial stress in the structure, the initial stress matrix 𝐊𝜎 (also called the nonlinear stiffness) is also added to the eigenvalue problem. LS-DYNA Theory Manual Sparse Eigensolver The damping and stiffness terms are easily derived in matrix form once the cross product is expressed in matrix form. 𝛚 × 𝐫 = 𝛀𝐫 = ⎡ 𝜔𝑧 ⎢⎢ −𝜔𝑦 𝜔𝑥 ⎣ −𝜔𝑧 𝜔𝑦 ⎤ −𝜔𝑥 ⎥⎥ 0 ⎦ { }. The linearized equation for vibration is 𝐌𝐮̈ + 𝐂𝐮̇ + [𝐊 + 𝐊σ]𝐮 = −𝐌{𝛀𝐮̇ + 𝛀2𝐮}. (40.4) (40.5) Rewriting this equation into the traditional form for eigenvalue analysis produces: 𝐌𝐮̈ + 𝐂R𝐮̇ + 𝐊R𝐮 = 0 𝐂R = 𝐂 + 𝐌𝛀 𝐌𝐮̈ + 𝐂R𝐮̇ + 𝐊R𝐮 = 0. (40.6) The inertial contribution to the damping matrix is not symmetric, nor does it fulfill the requirements for Rayleigh damping, and therefore the resulting eigenvectors and eigenvalues are complex. The inertial term to the stiffness matrix is, however, symmetric and it softens the structure, thereby reducing its natural frequencies. If the damping term is omitted, the matrices are real and symmetric, and the resulting eigenvalue problem may be solved with the standard eigenvalue methods. The natural frequencies won’t be correct, but they are typically close enough to the complex solution that they can be used for initial design calculations. LS-DYNA Theory Manual Boundary Element Method 41 Boundary Element Method LS-DYNA can be used to solve for the steady state or transient fluid flow about a body using a boundary element method. The method is based on the work of Maskew [1987], with the extension to unsteady flow with arbitrary body motion following the work of Katz and Maskew [1988]. The theory which underlies the method is restricted to inviscid, incompressible, attached fluid flow. The method should not be used to analyze flows where shocks or cavitation are present. In practice the method can be successfully applied to a wider class of fluid flow problems than the assumption of inviscid, incompressible, attached flow would imply. Many flows of practical engineering significance have large Reynolds numbers (above 1 million). For these flows the effects of fluid viscosity are small if the flow remains attached, and the assumption of zero viscosity may not be a significant limitation. Flow separation does not necessarily invalidate the analysis. If well-defined separation lines exist on the body, then wakes can be attached to these separation lines and reasonable results can be obtained. The Prandtl-Glauert rule can be used to correct for non-zero Mach numbers in air, so the effects of aerodynamic compressibility can be correctly modeled (as long as no shocks are present). 41.1 Governing Equations The partial differential equation governing inviscid, incompressible fluid flow is given by LaPlace’s equation ∇2𝛷 = 0, (41.1) where 𝛷 is the velocity potential (a scalar function). The fluid velocity anywhere in the flow field is equal to the gradient of 𝛷. The boundary condition on this partial differntial equation is provided by the condition that there must be no flow in the direction normal to the surface of the body. Note that time does not appear in Equation Boundary Element Method LS-DYNA Theory Manual (41.1). This is because the assumption of incompressibility implies an infinite sound speed; any disturbance is felt everywhere in the fluid instantaneously. Although this is not true for real fluids, it is a valid approximation for a wide class of low-speed flow problems. Equation (41.1) is solved by discretizing the surface of the body with a set of quadrilateral or triangular surface segments (boundary elements). Each segment has an associated source and doublet strength. The source strengths are computed from the free-stream velocity, and the doublet strengths are determined from the boundary condition. By requiring that the normal component of the fluid velocity be zero at the center of each surface segment, a linear system of equations is formed with the number of equations equal to the number of unknown doublet strengths. When this system is solved, the doublet strengths are known. The source and doublet distributions on the surface of the body then completely determine the flow everywhere in the fluid. The linear system for the unknown doublet strengths is shown in Equation (1.2). [mic]{𝜇} = {rhs}. (41.2) In this equation μ are the doublet strengths, [mic is the matrix of influence coefficients which relate the doublet strength of a given segment to the normal velocity at another segment’s mid-point, and rhs is a right-hand-side vector computed from the known source strengths. Note that mic is a fully-populated matrix. Thus, the cost to compute and store the matrix increases with the square of the number of segments used to discretize the surface of the body, while the cost to factor this matrix increases with the cube of the number of segments. Users should keep these relations in mind when defining the surface segments. A surface of 1000 segments can be easily handled on most any computer, but a 10,000 segment representation would not be feasible on any but the most powerful supercomputers. 41.2 Surface Representation The surface of the body is discretized by a set of triagular or quadrilateral surface segments. The best fluid-structure interaction results will be obtained if the boundary element segments coincide with, and use identical nodes as, the structural segments used to define the body. An input format has been implemented to make this easy if thin shell elements are used to define the structure . Using the same nodes to define the boundary elements and the structure guarantees that the boundary elements follow the structure as it deforms, and provides a means for the fluid pressure to load the structure. LS-DYNA Theory Manual Boundary Element Method normal node 4 node 3 node 1 node 2 Figure 41.1. Counter-clockwise ordering of nodes when viewed from fluid looking towards solid provides unit normal vector pointing into the fluid. The nodes used to define the corners of the boundary element segments must be ordered to provide a normal vector which points into the fluid (Figure 41.1). Triangular segments are specified by using the same node for the 3rd and 4th corner of the segment (the same convention used for shell elements in LS-DYNA). Very large segments can be used with no loss of accuracy in regions of the flow where the velocity gradients are small. The size of the elements should be reduced in areas where large velocity gradients are present. Finite-precision arithmetic on the computer will cause problems if the segment aspect ratios are extremely large (greater than 1000). The most accurate results will be obtained if the segments are rectangular, and triangular segments should be avoided except for cases where they are absolutely required. The fluid velocities (and, therefore, the fluid 41.3 The Neighbor Array pressures) are determined by the gradient of the velocity potential. On the surface of the body, this can be most easily computed by taking derivatives of the doublet distribution on the surface. These derivatives are computed using the doublet strengths on the boundary element segments. The “Neighbor Array” is used to specify how the gradient is computed for each boundary element segment. Thus, accurate results will not be obtained unless the neighbor array is correctly specified by the user. Each boundary element segment has 4 sides . Side 1 connects the 1st and 2nd nodes, side 2 connects the 2nd and 3rd nodes, etc. The 4th side is null for triangular segments. Boundary Element Method LS-DYNA Theory Manual node 4 side 3 side 4 node 3 side 2 side 1 node 1 node 2 Figure 41.2. Each segment has 4 sides. For most segments the specification of neighbors is straightforward. For the typical case a rectangular segment is surrounded by 4 other segments, and the neighbor array is as shown in Figure 41.3. A biquadratic curve fit is computed, and the gradient is computed as the analytical derivative of this biquadratic curve fit evaluated at the center of segment j. There are several situations which call for a different specification of the neighbor array. For example, boundary element wakes result in discontinuous doublet distributions, and the biquadratic curve fit should not be computed across a wake. Figure 41.4 illustrates a situation where a wake is attached to side 2 of segment 𝑗. For this situation two options exist. If neighbor (2, 𝑗) is set to zero, then a linear computation of the gradient in the side 2 to side 4 direction will be made using the difference between the doublet strengths on segment 𝑗 and segment neighbor (4, 𝑗). By specifying neighbor (2, 𝑗) as a negative number the biquadratic curve fit will be retained. The curve fit will use segment 𝑗, segment neighbor (4, 𝑗), and segment – neighbor (2, 𝑗); which is located on the opposite side of segment neighbor (4, 𝑗) as segment 𝑗. The derivative in the side 2 to side 4 direction is then analytically evaluated neighbor (3, j) neighbor(4, j) side 4 side 3 segment j side 1 neighbor (2, j) side 2 neighbor (1, j) Figure 41.3. Typical neighbor specification. LS-DYNA Theory Manual Boundary Element Method -neighbor (2, j) neighbor (4, j) segment j side 4 side 2 Figure 41.4. If neighbor (2, 𝑗) is a negative number it is assumed to lie on the opposite side of neighbor (4, 𝑗) as segment 𝑗. at the center of segement j using the quadratic curve fit of the doublet strengths on the three segments shown. A final possibility is that no neighbors at all are available in the side 2 to side 4 direction. In this case both neighbor (2, 𝑗) and neighbor (4, 𝑗) can be set to zero, and the gradient in that direction will be assumed to be zero. This option should be used with caution, as the resulting fluid pressures will not be accurate for three-dimensional flows. However, this option is occaisionally useful where quasi-two dimensional results are desired. All of the above options apply to the side 1 to side 3 direction in the obvious ways. For triangular boundary element segments side 4 is null. Gradients in the side 2 to side 4 direction can be computed as described above by setting neighbor (4, 𝑗) to zero (for a linear derivative computation) or to a negative number (to use the segment on the other side of neighbor (2, 𝑗) and a quadratic curve fit). There may also be another triangular segment which can be used as neighbor (4, 𝑗) . Boundary Element Method LS-DYNA Theory Manual 41.4 Wakes Wakes should be attached to the boundary element segments at the trailing edge of a lifting surface (such as a wing, propeller blade, rudder, or diving plane). Wakes should also be attached to known separation lines (such as the sharp leading edge of a delata wing at high angles of attack). Wakes are required for the correct computation of surface pressures for these situations. As described above, two segments on opposite sides of a wake should never be used as neighbors. Correct specification of the wakes is required for accurate results. Wakes convect with the free-stream velocity. The number of segments in the wake is controlled by the user, and should be set to provide a total wake length equal to 5-10 times the characteristic streamwise dimension of the surface to which the wake is attached. For example, if the wake is attached to the trailing edge of a wing whose chord is 1, then the total length of the wake should at least 5, and there is little point in making it longer than 10. Note that each wake segment has a streamwise length equal to the magnitude of the free stream velocity times the time increment between calls to the Boundary Element Method routine. This time increment is the maximum of the LS- DYNA time step and DTBEM specified on Card 1 of the BEM input. The influence coefficients for the wake segments must be recomputed for each call to the Boundary Element Method, but these influence coefficients do not enter into the matrix of influence coefficients which must be factored. 41.5 Execution Time Control The Boundary Element Method will dominate the total execution time of a LS- DYNA calculation unless the parameters provided on Card 1 of the BEM input are used to reduce the number of calls to the BEM. This can usually be done with no loss in neighbor(4, j) segment j side 2 Figure 41.5. Sometimes another triangular boundary element segment can be used as neighbor(4,j). accuracy since the characteristic time of the structural dynamics and the fluid flow are LS-DYNA Theory Manual Boundary Element Method so different. For example, the characteristic time in LS-DYNA is given by the characteristic length of the smallest structural element divided by the speed of sound of the material. For typical problems this characteristic time might be on the order of microseconds. Since the fluid is assumed to be incompressible (infinite speed of sound), the characteristic time of the fluid flow is given by the streamwise length of the smallest surface (e.g. a rudder) divided by the fluid velocity. For typical problems this characteristic time might be on the order of milliseconds. Thus, for this example, the boundary element method could be called only once for every 1000 LS-DYNA iterations, saving an enormous amount of computer time. The parameter DTBEM on Card 1 of the BEM input is used to control the time increment between calls to the boundary element method. The fluid pressures computed during the last call to the BEM will continue to be used for subsequent LS- DYNA iterations until DTBEM has elapsed. A further reduction in execution time may be obtained for some applications using the input parameter IUPBEM. This parameter controls the number of calls to the BEM routine between computation (and factorization) of the matrix of influence coefficients (these are time-consuming procedures). If the motion of the body is entirely rigid body motion there is no need to recompute and factor the matrix of influence coefficients, and the execution time of the BEM can be significantly reduced by setting IUPBEM to a very large number. For situations where the motion of the body is largely rigid body motion with some structural deformation an intermediate value (e.g. 10) for IUPBEM can be used. It is the user’s responsibility to verify the accuracy of calculations obtained with IUPBEM greater than 1. The final parameter for controlling the execution time of the boundary element method is FARBEM. The routine which calculates the influence coefficients switches between an expensive near-field and an inexpensive far-field calculation depending on the distance from the boundary element segment to the point of interest. FARBEM is a nondimensional parameter which determines where the far-field boundary lies. Values of FARBEM of 5 and greater will provide the most accurate results, while values as low as 2 will provide slightly reduced accuracy with a 50% reduction in the time required to compute the matrix of influence coefficients. 41.6 Free-Stream Flow The free-stream flow is specified in the second card of input. The free-stream velocity is assumed to be uniform. The free-stream static pressure is assumed to be uniform, and can be used to load the structure for hydrostatic pressure. If the structure has an internal pressure, the free-stream static pressure should be set to the difference between the external and internal static pressures. The Mach number can be used to Boundary Element Method LS-DYNA Theory Manual correct for the effect of compressibility in air (as long as no shocks are present). Following the Prandtl-Glauert correction, the pressures due to fluid flow are increased as follows 𝑑𝑝corrected = 𝑑𝑝uncorrected √1 − 𝑀2 (41.3) where M is the free-stream Mach number. Note that this correction is only valid for flows in a gas (it is not valid for flows in water). LS-DYNA Theory Manual SPH 42 SPH Smoothed Particle Hydrodynamics (SPH) is an N-body integration scheme developed by Lucy, Gingold and Monaghan [1977]. The method was developed to avoid the limitations of mesh tangling encountered in extreme deformation problems with the finite element method. The main difference between classical methods and SPH is the absence of a grid. Therefore, the particles are the computational framework on which the governing equations are resolved. This new model requires a new calculation method, which is briefly explained in the following. 42.1 SPH Formulation 42.1.1 Definitions The particle approximation of a function is: Πℎ𝑓 (𝑥) = ∫ 𝑓 (𝑦)𝑊(𝑥 − 𝑦, ℎ)𝑑𝑦, where 𝑊 is the kernel function. The Kernel function 𝑊 is defined using the function 𝜃 by the relation: 𝑊(𝐱, ℎ) = ℎ(𝐱)𝑑 𝜃(𝐱). (42.1) (42.2) where 𝑑 is the number of space dimensions and ℎ is the so-called smoothing length which varies in time and in space. 𝑊(𝐱, ℎ) should be a centrally peaked function. The most common smoothing kernel used by the SPH community is the cubic B-spline which is defined by choosing 𝜃 as: SPH LS-DYNA Theory Manual 𝜃(𝑢) = 𝐶 × ⎧ {{{ ⎨ {{{ ⎩ 1 − 𝑢2 + 𝑢3 for |𝑢| ≤ 1 (2 − 𝑢)3 for 1 ≤ |𝑢| ≤ 2 for 2 < |𝑢| (42.3) where C is a constant of normalization that depends on the number of space dimensions. The SPH method is based on a quadrature formula for moving particles ((𝐱𝑖(𝑡)) 𝑖 ∈ {1. . 𝑁}, where 𝐱𝑖(𝑡) is the location of particle 𝑖, which moves along the velocity field v. The particle approximation of a function can now be defined by: Πℎ𝑓 (𝐱𝑖) = ∑ 𝑤𝑗𝑓 (𝐱𝑖)𝑊(𝐱𝑖 − 𝐱𝑗, ℎ) , 𝑗=1 (42.4) where 𝑤𝑗 = proportionally to the divergence of the flow. 𝑚𝑗 𝜌𝑗 is the “weight” of the particle. The weight of a particle varies The SPH formalism implies a derivative operator. A particle approximation for the derivative operator must be defined. Before giving the definition of this approximation, we define the gradient of a function as: ∇𝑓 (𝑥) = ∇𝑓 (𝑥) − 𝑓 (𝑥)∇1(𝑥), (42.5) where 1 is the unit function. Starting from this relation, we can define the particle approximation to the gradient of a function: Πℎ∇𝑓 (𝐱𝑖) = ∑ 𝑗=1 𝑚𝑗 𝜌𝑗 , [𝑓 (𝐱𝑗)𝐴𝑖𝑗 − 𝑓 (𝐱𝑖)𝐴𝑖𝑗] (42.6) where 𝐴𝑖𝑗 = 1 ℎ𝑑+1 𝜃′( ||𝐱𝑖−𝐱𝑗|| ). We can also define the particle approximation of the partial derivative ∂ ∂𝑥𝛼: Πℎ( ∂𝑓 ∂𝑥𝛼)(𝐱𝑖) = ∑ 𝑤𝑗 𝑗=1 𝑓 (𝐱𝑗𝐴𝛼(𝐱𝑖, 𝐱𝑗), (42.7) where 𝐀 is the operator defined by: 𝐀(𝐱𝑖, 𝐱𝑗) = ℎ𝑑+1(𝐱𝑖,𝐱𝑗) (𝐱𝑖−𝐱𝑗) |∣𝐱𝑖−𝐱𝑗∣| 𝜃′ ( |∣𝐱𝑖−𝐱𝑗∣| ℎ(𝐱𝑖,𝐱𝑗)), 𝐴𝛼 is the component 𝛼 of the 𝐀 vector. LS-DYNA Theory Manual 42.1.2 Discrete Form of Conservation Equations We are looking for the solution of the equation: 𝐿𝑣(𝜙) + div𝐅(𝐱, 𝑡, 𝜙) = 𝑆, SPH (42.8) where 𝜙 ∈ 𝑅𝑑 is the unknown, 𝐅𝛽 with 𝛽 ∈ {1. . 𝑑} represents the conservation law and 𝐿𝑣 is the transport operator defined by: 𝐿𝑣: 𝜙 → 𝐿𝑣(𝜙) = ∂𝜙 ∂𝑡 + ∑ 𝑙=1 ∂(𝐯𝑙𝜙) . ∂𝑥𝑙 (42.9) The strong formulation approximation: In the search of the strong solution, the equation is kept at its initial formulation. The discrete form of this problem implies the definition of the operator of derivation 𝐷 defined by: 𝐷: 𝜙 → 𝐷𝜙(𝑥) = ∇𝜙(𝑥) − 𝜙(𝑥)∇1(𝑥). The particle approximation of this operator is: 𝐷ℎ𝜙(𝐱𝑖) = ∑ 𝑤𝑗(𝜙(𝐱𝑗) − 𝜙(𝐱𝑖))𝐴𝑖𝑗 , 𝑗=1 where 𝐴𝑖𝑗 is defined previously. (42.10) (42.11) Finally, the discrete form of the strong formulation is written: 𝑑𝑡 (𝑤𝑖𝜙(𝐱𝑖)) + 𝑤𝑖𝐷ℎ𝐹(𝐱𝑖) = 𝑤𝑖𝑆(𝐱𝑖), (42.12) But this form is not conservative; therefore the strong formulation is not numerically acceptable. Thus, we are compelled to use the weak form. The weak formulation approximation: In the weak formulation, the adjoint of the 𝐿𝑣 operator is used: ∗: 𝜙 → 𝐿𝑣 𝐿𝑣 ∗(𝜙) = ∂𝜙 ∂𝑡 + ∑ 𝑣𝑙 𝑙=1 ∂𝜙 ∂𝑥𝑙 . (42.13) The discrete form of this operator corresponds to the discrete formulation of the adjoint of 𝐷ℎ,𝑠: 𝐷ℎ,𝑠 ∗ 𝜙(𝐱𝑖) = ∑ 𝑤𝑗(𝜙(𝐱𝑖 𝑗=1 )𝐴𝑖𝑗 − 𝜙(𝐱𝑗)𝐴𝑗𝑖). (42.14) A discrete adjoint operator for the partial derivative is also necessary, and is taken to be the 𝛼 − 𝑡ℎ component of the operator: SPH LS-DYNA Theory Manual 𝐷𝛼 ∗𝜙(𝐱𝑖) = ∑ 𝑤𝑗 𝜙(𝐱𝑗)𝐴𝛼(𝐱𝑖, 𝐱𝑗) − 𝑤𝑗𝜙(𝐱𝑖)𝐴𝛼(𝐱𝑗, 𝐱𝑖) (42.15) 𝑗=1 These definitions are leading to a conservative method. Hence, all the conservative equations encountered in the SPH method will be solved using the weak form. 42.1.3 Applications to Conservation Equations With the definitions explained above, the conservation equations can now be written in their discrete form. Momentum conservation equation: 𝑑𝐯𝛼 𝑑𝑡 (𝐱𝑖(𝑡)) = 𝜌𝑖 ∂(𝜎 𝛼𝛽) ∂𝑥𝑖 (𝐱𝑖(𝑡)), where 𝛼, 𝛽 are the space indices. The particle approximation of the weak form of this equation is: ⎜⎛𝜎 𝛼,𝛽(𝐱𝑖) 2 𝐴𝑖𝑗 − 𝜌𝑖 ⎝ 𝜎 𝛼,𝛽(𝐱𝑗) 𝜌𝑗 (𝐱𝑖) = ∑ 𝑚𝑗 𝑑𝐯𝛼 𝑑𝑡 ⎟⎞. ⎠ 𝐴𝑗𝑖 𝑗=1 Energy conservation equation: 𝑑𝐸 𝑑𝑡 = − ∇𝐯. (42.16) (42.17) (42.18) The particle approximation of the weak form of this equation is: 𝑑𝐸 𝑑𝑡 (𝐱𝑖) = − 𝑃𝑖 2 ∑ 𝑚𝑗 𝜌𝑖 𝑗=1 (𝑣(𝐱𝑗) − 𝑣(𝐱𝑖))𝐴𝑖𝑗. (42.19) 42.1.4 Formulation Available in LS-DYNA It is easy from the general formulation displayed in Equation (42.14) to extend the SPH formalism to a set of equations of discretization for the momentum equation. For example, if we choose the smoothing function to be symmetric, this can lead to the following equation: 𝑑𝐯𝛼 𝑑𝑡 (𝐱𝑖) = ∑ 𝑚𝑗 𝑗=1 ⎜⎛𝜎 𝛼,𝛽(𝐱𝑖) 2 + 𝜌𝑖 ⎝ 𝜎 𝛼,𝛽(𝐱𝑗) 𝜌𝑗 ⎟⎞ 𝐴𝑖𝑗. ⎠ (42.20) LS-DYNA Theory Manual SPH This is what we call the “symmetric formulation”, which is chosen in the *CONTROL_SPH card (IFORM = 2). Another possible choice is to define the momentum equation by: ⎜⎛𝜎 𝛼,𝛽(𝐱𝑖) 𝜌𝑖𝜌𝑗 ⎝ 𝜎 𝛼,𝛽(𝐱𝑗) 𝜌𝑖𝜌𝑗 (𝐱𝑖) = ∑ 𝑚𝑗 𝑑𝐯𝛼 𝑑𝑡 ⎟⎞. ⎠ 𝐴𝑖𝑗 − 𝐴𝑗𝑖 𝑗=1 (42.21) This is the “fluid formulation” invoked with IFORM = 5 which gives better results than other SPH formulations when fluid material are present, or when material with very different stiffness are used. 42.2 Sorting In the SPH method, the location of neighboring particles is important. The sorting consists of finding which particles interact with which others at a given time. A bucket sort is used that consists of partitioning the domain into boxes where the sort is performed. With this partitioning the closest neighbors will reside in the same box or in the closest boxes. This method reduces the number of distance calculations and therefore the CPU time. 42.3 Artificial Viscosity The artificial viscosity is introduced when a shock is present. Shocks introduce discontinuities in functions. The role of the artificial viscosity is to smooth the shock over several particles. To take into account the artificial viscosity, an artificial viscous pressure term Π𝑖𝑗 [Monaghan & Gingold 1983] is added such that: 𝑝𝑖 → 𝑝𝑖 + Π𝑖𝑗, (42.22) where Π𝑖𝑗 = 1 𝜌̅𝑖𝑗 (−𝛼𝜇𝑖𝑗𝑐 ̅𝑖𝑗 + 𝛽𝜇𝑖𝑗 2 ). The notation 𝑋̅̅̅̅̅𝑖𝑗 = 1 the adiabatic sound speed, and 2 (𝑋𝑖 + 𝑋𝑗) has been used for median between 𝑋𝑖 and 𝑋𝑗, 𝑐 is 𝑣𝑖𝑗𝑟𝑖𝑗 2 + 𝜂2 𝑟𝑖𝑗 0 Here, 𝑣𝑖𝑗 = (𝑣𝑖 − 𝑣𝑗), and 𝜂2 = 0.01ℎ̅ 𝜇𝑖𝑗 = {⎧ {⎨ ⎩ ℎ̅ 𝑖𝑗 if 𝑣𝑖𝑗𝑟𝑖𝑗 < 0 otherwise (42.23) 2 which prevents the denominator from vanishing. 𝑖𝑗 SPH LS-DYNA Theory Manual 42.4 Time Integration We use a simple and classical first-order scheme for integration. The time step is determined by the expression: 𝛿𝑡 = 𝐶CFL𝑀𝑖𝑛𝑖 ( ℎ𝑖 𝑐𝑖 + 𝑣𝑖 ), (42.24) where the factor 𝐶CFL is a numerical constant. The calculation cycle is: Start Velocity/positions LS-DYNA Accelerations LS-DYNA contact, boundary conditions LS-DYNA Smoothing length SPH Sorting SPH Particles forces SPH Density, strain rates SPH Pressure, thermal energy, stresses LS-DYNA 42.5 Initial Setup Initially, we have a set of particles with two kinds of properties: physical and geometrical properties. Physical Properties: LS-DYNA Theory Manual SPH The mass, density, constitutive laws are defined in the ELEMENT_SPH and the PART cards. Geometrical Properties: The geometrical properties of the model concern the way particles are initially placed. Two different parameters are to be fixed: Δ𝑥𝑖 lengths and the CSLH coefficient. These parameters are defined in the SECTION_SPH card. A proper SPH mesh must satisfy the following conditions: it must be as regular as possible and must not contain too large variations. For instance, if we consider a cylinder SPH mesh, we have at least two possibilities: The mesh number 2 includes too many inter-particle distance discrepancies. Therefore, the first mesh, more uniform, is better. Finite element coupling Coupling finite elements and SPH elements is realized by using contact algorithms. Users can choose any “nodes_to_surface” contact type where the slave part is defined with SPH elements and the master part is defined with finite elements. LS-DYNA Theory Manual Element-Free Galerkin 43 Element-Free Galerkin Mesh-free methods, which construct the approximation entirely in terms of nodes, permit reduced restriction in the discretization of the problem domain and are less susceptible to distortion difficulties than finite elements. For a variety of engineering problems with extremely large deformation, moving boundaries or discontinuities, mesh-free methods are very attractive. The two most commonly used approximation theories in mesh-free methods are the moving least-squares (MLS) approximation in the Element-free Galerkin (EFG) method [Belytschko et al. 1994], and the reproducing kernel (RK) approximation in the reproducing kernel particle method (RKPM) [Liu et al. 1995]. Since these two methods lead to an identical approximation when monomial basis functions are used, the MLS approximation is used as a basis to formulate the mesh-free discrete equations in this section. 43.1 Moving least-squares The Element-free Galerkin method uses the moving least-squares approximation to construct the numerical discretization. The discrete MLS approximation of a function 𝑢(𝐱), denoted by 𝑢ℎ(𝐱), is constructed by a combination of the monomials as 𝑢ℎ(𝐱) = ∑ 𝐻𝑖(𝐱)𝑏𝑖(𝐱) ≡ 𝐇T(𝐱)𝐛(𝐱) , 𝑖=1 (43.1) where 𝑛 is the order of completeness in this approximation, the monomial 𝐻𝑖(𝐱) are basis functions, and 𝑏𝑖(𝐱) are the coefficients of the approximation. The coefficients 𝑏𝑖(𝐱) at any point 𝐱 are depending on the sampling points 𝐱𝐼 that are collected by a weighting function 𝑤𝑎(𝐱 − 𝐱𝐼). This weighting function is defined to have a compact support measured by ‘a’, i.e., the sub-domain over which it is nonzero is small relative to the rest of the domain. Each sub-domain ΔΩ𝐼 is associated with a node 𝐼. The most commonly used sub-domains are disks or balls. A typical numerical model is shown in Figure 43.1. Element-Free Galerkin LS-DYNA Theory Manual Figure 43.1. Graphical representation of mesh-free discretization In this development, we employ the cubic B-spline kernel function as the weighting function: − 4 ( ) + 4 ( ‖𝐱 − 𝐱𝐼‖ ‖𝐱 − 𝐱𝐼‖ − 4 ( ) + 4 ( ) ‖𝐱 − 𝐱𝐼‖ ‖𝐱 − 𝐱𝐼‖ ) − ( ‖𝐱 − 𝐱𝐼‖ ) 𝑤𝑎(𝐱 − 𝐱𝐼) = ⎧2 { { { { { ⎨ { { { { { ⎩ for 0 ≤ for < ‖𝐱 − 𝐱𝐼‖ ‖𝐱 − 𝐱𝐼‖ ≤ ≤ 1 otherwise ⎫ } } } } } ⎬ } } } } } ⎭ (43.2) The moving least-squares technique consists in minimizing the weighted L2- Norm NP 𝐽 = ∑ Wa(𝐱) 𝐼=1 ] (𝐱 − 𝐱𝐼) [∑ 𝐻𝑖(𝐱)𝑏𝑖(𝐱) − 𝑢(𝐱𝐼) , 𝑖=1 (43.3) where NP is the number of nodes within the support of 𝐱 for which the weighting function 𝑤𝑎(𝐱 − 𝐱𝐼) ≠ 0. Equation (39.3) can be written in the form 𝐽 = (𝐇𝐛 − 𝐮)TWa(𝐱)(𝐇𝐛 − 𝐮), where 𝐮T = (𝑢1, 𝑢2, ⋯ 𝑢NP), (43.4) (43.5) LS-DYNA Theory Manual Element-Free Galerkin 𝐇 = {𝐇(𝐱1)}T ⎤ ⎡ , ⋯ ⎥ ⎢ {𝐇(𝐱NP)}T⎦ ⎣ {𝐇(x𝑖)}T = {𝐻1(𝐱𝑖), … 𝐻𝑛(𝐱𝑖)}, 𝐖a = diag[𝑤𝑎(𝐱 − 𝐱1), ⋯ , 𝑤𝑎(𝐱 − 𝐱NP)]. To find the coefficients 𝐛 we obtain the extremum of 𝐽 by ∂𝐽 ∂b = 𝐌[n](𝐱)𝐛(𝐱) − 𝐁(𝐱)𝐮 = 0, where 𝐌[𝑛](𝐱) is called the moment matrix of 𝑤𝑎(𝐱 − 𝐱𝐼) and is given by So we have 𝐌[n](𝐱) = 𝐇T𝐖a(𝐱)𝐇, 𝐁(𝐱) = 𝐇T𝐖a(𝐱). 𝐛(𝐱) = 𝐌[n]−1 (𝐱)𝐁(𝐱)𝐮. (43.6) (43.7) (43.8) (43.9) (43.10) (43.11) (43.12) For 𝐌[𝑛](𝐱) to be invertible, the support of 𝑤𝑎(𝐱 − 𝐱) needs to be greater than a minimum size that is related to the order of basis functions. Using the solution of Equations (43.1), (43.10), (43.11) and (43.12), the EFG approximation is obtained by NP 𝑢ℎ(𝐱) = ∑ Ψ𝐼(𝐱)𝑢𝐼 𝐼=1 , where the EFG shape functions Ψ𝐼(𝐱) are given by Ψ𝐼(𝐱) = 𝐇T(𝐱)𝐌[n]−1 (𝐱)𝐁(𝐱), and 𝚿𝐼(𝐱) are nth-order complete, i.e. 𝑁𝑃 ∑ Ψ𝐼(𝐱)𝑥1𝐼 𝐼=1 𝑞 = 𝑥1 𝑥2𝐼 𝑝𝑥2 𝑞 for 𝑝 + 𝑞 = 0, ⋯ 𝑛. (43.13) (43.14) (43.15) 43.2 Integration constraint and strain smoothing The convergence of the Galerkin method for a partial differential equation is determined by approximation for the unknowns and the numerical integration of the weak form. EFG shape functions with linear consistency can be obtained from MLS approximation with linear basis functions. The employment of linearly consistent mesh-free shape functions in the Galerkin approximation, however, does not guarantee Element-Free Galerkin LS-DYNA Theory Manual a linear exactness in the solution of the Galerkin method. It has been shown by Chen et al. [2001] that two integration constraints are required for the linear exactness solution in the Galerkin approximation. NIT ∑ ∇ΨI(x̂L)AL 𝐿=1 = 0 for {𝐼: supp(Ψ𝐼) ∩ Γ = 0}, (43.16) NIT ∑ ∇ΨI(x̂L)AL 𝐿=1 NITh = ∑ nΨ𝐼(x̃𝐿)𝑠𝐿 𝐿=1 for {𝐼: supp(Ψ𝐼) ∩ Γℎ ≠ 0}. (43.17) where Γℎ is the natural boundary, Γ is the total boundary, 𝐧 is the surface normal on Γℎ, x̂𝐿 and 𝐴𝐿 are the spatial co-ordinate and weight of the domain integration point, respectively, x̃𝐿 and 𝑠𝐿 are the spatial co-ordinate and weight of the domain of natural boundary integration point, respectively, NIT is the number of integration points for domain integration and NITh is the number of integration points for natural boundary integration. A strain smoothing method proposed by Chen and Wu [1998] as a regularization for material instabilities in strain localization was extended in their nodal integration method [Chen et al, 2001] to meet the integration constraints. Here, we adopt the similar concept for the domain integration. If starts with a strain smoothing at the representative domain of a Gauss point by ∇̃𝑢𝑖 ℎ(x𝐿) = 𝐴𝐿 ∫ ∇𝑢𝑖 Ω𝐿 ℎ(x𝐿) 𝑑Ω, 𝐴𝐿 = ∫ 𝑑Ω Ω𝐿 , (43.18) where Ω𝐿 is a representative domain at each Guass point and ∇̃ is the smoothed gradient operator. By applying divergence theorem to Equation (43.18) to yield ∇̃𝑢𝑖 ℎ(x𝐿) = 𝐴𝐿 ∫ n𝑢𝑖 Γ𝐿 ℎ(x𝐿) 𝑑Γ, (43.19) where Γ𝐿 is the boundary of the representative domain of Guass point L. Introducing EFG shape functions into Equation (25.22) yields ∇̃𝑢𝑖 ℎ(x𝐿) = ∑ 𝐴𝐿 ∫ Ψ𝐼(x)n Γ𝐿 𝑑Γ ⋅ 𝑑𝑖𝐼 ≡ ∑ ∇̃Ψ𝐼(x𝐿) ⋅ 𝑑𝑖𝐼 . (43.20) It can be shown that the smoothed EFG shape function gradient ∇̃Ψ𝐼(xL) meets the integration constraints in Equations (43.16) and (43.17) regardless of the numerical integration employed. LS-DYNA Theory Manual Element-Free Galerkin 43.3 Lagrangian strain smoothing for path-dependent problems To avoid the tensile instability caused by the Eulerian kernel functions, the Lagrangian kernel functions are implemented in the current LS-DYNA. To introduce the Lagrangian EFG shape function into the approximation of a path-dependent problem, the strain increment Δ𝑢𝑖,𝑗 is computed by Δ𝑢𝑖,𝑗 = ∂Δ𝑢𝑖 ∂𝑥𝑗 = ∂Δ𝑢𝑖 ∂𝑋𝑘 −1. −1 = Δ𝐹𝑖𝑘𝐹𝑘𝑗 𝐹𝑘𝑗 The strain smoothing of Δ𝑢𝑖,𝑗 at a material pointx𝐿is computed by −1(x𝐿), Δ𝑢̃𝑖,𝑗(x𝐿) = Δ𝐹̃𝑖𝑘(x𝐿)𝐹̃ 𝑘𝑗 (43.21) (43.22) where 𝐹̃𝑖𝑗(x𝐿) is the Langrangian strain smoothing of deformation gradient and is given by 𝐹̃𝑖𝑗(x𝐿) = 𝐴𝐿 ℎ𝑁𝑗 ∫ 𝑢𝑖 Γ𝐿 𝑑Γ + δ𝑖𝑗. (43.23) 43.4 Galerkin approximation for explicit dynamic computation The strong form of the initial/boundary value problem for elasto-dynamics is as follows: ρ𝐮̈ = ∇ ⋅ 𝛔 + 𝐟b in Ω, (43.24) with the divergence operator ∇, the body force 𝐟𝑏, mass density ρ ,and with the boundary conditions: and initial conditions 𝐮 = 𝐮0 on Γ𝑢 𝛔 ⋅ 𝐧 = 𝐡 on Γℎ, 𝐮(𝐗, 0) = 𝐮0(𝐗) 𝐮̇(X, 0) = 𝐮̇0(𝐗). (43.25) (43.26) To introduce the Lagrangian strain smoothing formulation into the Galerkin approximation, an assumed strain method is employed. The corresponding weak form becomes: Element-Free Galerkin LS-DYNA Theory Manual ∫ ρδ𝐮 ⋅ Ω𝑥 𝐮̈dΩ + ∫ δ𝛆̃ Ω𝑥 : 𝛔dΩ = ∫ δ𝐮 ⋅ Ω𝑥 𝐟bdΩ + ∫ δ𝐮 ⋅ Γℎ 𝐡dΓ. (43.27) Following the derivation for explicit time integration, the equations to be solved have the form where δ𝐮T𝐌𝐮̈ = δ𝐮T𝐑, 1𝐼,𝑑 ̈ 𝐮̈𝐼 = [𝑑 ̈ 2𝐼, 𝑑 ̈ 𝑀𝐼𝐽 = ∫ ρΨ𝐼(𝐱)Ψ𝐽(𝐱)𝑑Ω = 3𝐼]𝑇 Ω𝑥 R𝐼 = ∫ 𝐁̃𝐼 Ω𝑥 𝑇(𝐱) ⋅ 𝛔(𝐅̃)𝑑Ω ∫ ρ0Ψ𝐼(𝐗)Ψ𝐽(𝐗)𝑑Ω Ω𝑋 − [Ψ𝐼(x)𝐡]∣ Γℎ − ∫ Ψ𝐼(x)𝐟b𝑑Ω Ω𝑥 (43.28) (43.29) , where B̃𝐼 coefficient of the approximation or the “generalized” displacement. 𝑇(x) is the smoothed gradient matrix obtained from Equation (43.22), 𝑑𝑖𝐼 is the 43.5 Imposition of essential boundary condition In general, mesh-free shape functions Ψ𝐼 do not possess Kronecker delta properties of the standard FEM shape functions, i.e. Ψ𝐼(xJ) ≠ δ𝐼𝐽. (43.30) This is because, in general, the mesh-free shape functions are not interpolation functions. As a result, a special treatment is required to enforce essential boundary conditions. There are many techniques for mesh-free methods to impose the essential boundary condition. Here, we adopt the transformation method as originally proposed for the RKPM method by Chen et al. [1996]. Therefore, to impose the essential boundary conditions using kinematically admissible mesh-free shape functions by the transformation method, Equation (43.28) can be written as where or and δ𝐮̂T𝐌̂𝐮̈ = δ𝐮̂T𝐅̂int, 𝐮̂ = 𝐀𝐮; 𝐴𝐼𝐽 = Ψ𝐽(𝑋𝐼). 𝐮 = 𝐀−1𝐮̂, (43.31) (43.32) (43.33) LS-DYNA Theory Manual Element-Free Galerkin 𝐌̂ = 𝐀−T𝐌𝐀−1; 𝐅̂int = 𝐀−T𝐅int. (43.34) A mixed transformation method [Chen et al. 2000] is also considered as an alternative to impose the essential boundary conditions. The mixed transformation method is an improved transformation method that the coordinate transformation is only applied for the degrees of freedom associated with the essential and contact boundaries. The nodes are partitioned into three groups: a boundary group 𝐺𝐵1 which contains all the nodes subjected to kinematic constraints; group 𝐺𝐵2 which contains all the nodes whose kernel supports cover nodes in group 𝐺𝐵1; and internal group 𝐺𝐼 which contains the rest of nodes. Nodes numbers are re-arranged in the following order in the generalized displacement vector: u𝐵1 ⎤ ⎡ u𝐵2 ⎥ ⎢ u𝐼 ⎦ ⎣ where 𝐮𝐵1, 𝐮𝐵2 and 𝐮𝐼 are the generalized displacement vectors associated with groups 𝐺𝐵1, 𝐺𝐵2 and 𝐺𝐼 respectively. The transformation in Equation (43.32) is also re-arranged as 𝐮 = (43.35) 𝐮̂ = [𝐮̂𝐵 𝐮̂𝐼 ] [ΛBB ΛBI ΛIB ΛII ] [𝐮𝐵 𝐮𝐼 ] ≡ 𝚲̂𝐮, where 𝐮̂B = [û𝐵1 û𝐵2 ] ; 𝐮B = [u𝐵1 u𝐵2 = [Λ𝐼𝐵1 Λ𝐼𝐵2]. ] ; 𝚲BB = [ΛB1B1 ΛB1B2 ΛB2𝐵1 ΛB2B2 ] ; 𝚲BI = [ Λ𝐵2𝐼] ; 𝚲IB Here, we introduce a mixed displacement vector 𝐮∗, 𝐮∗ = [𝐮̂𝐵 𝐮𝐼 ] [ΛBB ΛBI ] [𝐮𝐵 𝐮𝐼 ] ≡ 𝚲∗𝐮, and Λ∗ and its inverse are: 𝚲∗ = [ΛBB ΛBI ] ; 𝚲∗−1 = [ΛBB−1 −ΛBB−1 ΛBI ]. Only the inversion of Λ𝐵𝐵is required in Equation (22.68.15). (43.36) (43.37) (43.38) (43.39) Using the mixed coordinates in Equation (43.38), the transformed discrete Equation (43.31) becomes δ𝐮∗T𝐌∗𝐮̈∗ = δ𝐮∗T𝐑∗, (43.40) where Element-Free Galerkin LS-DYNA Theory Manual 𝐌∗ = 𝐀∗−T𝐌𝐀∗−1; 𝐑∗ = 𝐀∗−T𝐑. (43.41) The computation in Equations (43.41) is much less intensive than that in Equation (43.31), especially when the number of boundary and contact nodes is much smaller than the number of interior nodes. 43.6 Mesh-free Shell The extension of explicit mesh-free solid analysis to shell analysis is described in this section. Two projection methods are developed to generate the shell mid-surface using the moving-least-squares approximations. A co-rotational, updated Lagrangian procedure is adopted to handle arbitrarily large rotations with moderate strain responses of the shell structures. A local boundary integration method in conjunction with the selective reduced integration method is introduced to enforce the linear exactness and relieve shear locking. 43.6.1 Mesh-free Shell Surface Representation Surface reconstruction from disorganized nodes is very challenging in three dimensions. The problem is ill posed, i.e., there is no unique solution. Lancaster et al. [1981] first proposed a fast surface reconstruction using moving least squares method. Their approach was then applied to the computational mechanics under the name ‘mesh-free method’. Implicitly, the mesh-free method uses a combination of smooth basis functions (primitives) to find a scalar function such that all data nodes are close to an iso-contour of that scalar function in a global sense. In reality, the shell surface construction using the 3D mesh-free method is inadequate. This is because the topology of the real surface can be very complicated in three dimensions. Without the information on the ordering or connectivity of nodes, the reconstructed surface will not be able to represent shell intersections, exterior boundaries and shape corners. In our development of mesh-free shells, we assume that a shell surface is described by a finite element mesh. This can be easily accomplished by converting a part of shell finite elements into mesh-free zone. With the connectivity of nodes provided by the finite element mesh, a shell surface can be reconstructed with mesh- free interpolation from the nodal positions 𝐱̅ = Ψ̃𝐼(𝐗)𝐱𝐼, (43.42) where 𝐱𝐼 is the position vector of the finite element node on the shell surface and Ψ̃𝐼(𝐗) is the mesh-free shape function. In the above surface representation, a 3D arbitrary shell surface needs to be projected to a 2D plane. Two approaches for the projection of mesh-free shell surface are used: LS-DYNA Theory Manual Element-Free Galerkin Projection Figure 43.2. Mesh-free shell global approach • Global parametric representation: The whole shell surface is projected to a parametric plane and the global parametric coordinates are obtained with a parameterization algorithm from the patch of finite elements. • Local projection representation: A local area of the shell is projected to a plane based on the existing element where the evaluated point is located. Global parametric approach In the global approach, a mesh-free zone with a patch of finite elements is mapped onto a parametric plane with an angle-based triangular flattening algorithm [Sheffer and de Sturler 2001], . The idea of this algorithm is to compute a projection that minimizes the distortion of the FE mesh angles. The mesh-free shape functions are defined in this parametric domain and given by Ψ̃𝐼(𝐗) = Ψ̃𝐼(𝜉 , 𝜂), (43.43) where (𝜉 , 𝜂) is the parametric coordinates corresponding to a point X. Local projection approach Different from the parameterization algorithm that constructs the surface globally, we reconstruct the surface locally by projecting the surrounding nodes onto one element. In the local projection method, nodes in elements neighboring the element where the evaluated point is located (for example, the element i in Figure 43.3) are projected onto the plane which the element defines (the “M-plane” in Figure 43.3). In this figure, (𝑥̂, 𝑦̂, 𝑧̂)𝑖 is a local system defined for each projected plane and (𝑥̅, 𝑦̅, 𝑧̅)𝐼 is a nodal coordinate system defined for each node where 𝑧̅ is the initial averaged normal direction. The mesh-free shape functions are then defined with those locally projected coordinates of the nodes Ψ𝐼(𝐗) = Ψ𝐼(𝑥̂, 𝑦̂). (43.44) Element-Free Galerkin LS-DYNA Theory Manual zI¯ M-plane yI¯ xI¯ ^ zi ^ yi M-plane ^ xi Figure 43.3. Mesh-free shell local projection However, the shape functions obtained directly above are non-conforming, i.e. Ψ𝐼(𝐗𝐽)∣ M−plane ≠ Ψ𝐼(𝐗𝐽)∣ N−plane . (43.45) When the shell structure degenerates to a plate, the constant stress condition cannot be recovered. To remedy this problem, an area-weighed smoothing across different projected planes is used to obtain the conforming shape functions that are given by Ψ̃𝐼(𝐗) = Ψ̃𝐼(𝑥̂, 𝑦̂) = NIE 𝑖=1 ∑ Ψ𝐼(𝑥̂𝑖, 𝑦̂𝑖)𝐴𝑖 𝑁𝐼𝐸 ∑ 𝐴𝑖 𝑖=1 . (43.46) where NIE is the number of surrounding projected planes that can be evaluated at point X, 𝑨𝒊 is the area of the element 𝑖, and (𝑥̂𝑖, 𝑦̂𝑖) is the local coordinates of point X in the projected plane 𝑖. With this smoothing technique, we can prove that the modified shape functions satisfy at least the partition of unity property in the general shell problems. This property is important for the shell formulation to preserve the rigid-body translation. When the shell degenerates to a plate, we can also prove that the shape functions obtained from this smoothing technique will meet the n-th order completeness condition as NP ∑ Ψ̃𝐼(𝐗)𝑋1𝐼 𝐼=1 𝑖 𝑋2𝐼 𝑗 𝑋3𝐼 = 𝑋1 𝑖 𝑋2 𝑗 𝑋3 𝑘, 𝑖 + 𝑗 + 𝑘 = 𝑛. (43.47) This is a necessary condition for the plate to pass the constant bending patch test. 43.6.2 Updated Lagrangian Formulation and Co-rotational Procedure The mesh-free shell formulation is based on the Mindlin-Reissner plate theory, thus the geometry and kinematical fields of the shell can be described with the reference LS-DYNA Theory Manual Element-Free Galerkin z^ ζV3 y^ x^ x¯ Figure 43.4. Geometry of a shell. surface and fiber direction. The modified Mindlin-Reissner assumption requires that the motion and displacement of the shell are linear in the fiber direction. Assume that the reference surface is the mid-surface of the shell, the global coordinates and displacements at an arbitrary point within the shell body are given by 𝐱 = 𝐱̅ + ζ 𝐕3, (43.48) where 𝐱̅ and 𝐮̅̅̅̅ are the position vector and displacement of the reference surface, respectively. 𝐕3 is the fiber director and 𝐔 is the displacement resulting from the fiber rotation . ℎ is the length of the fiber. 𝐮 = 𝐮̅̅̅̅ + ζ (43.49) 𝐔. With the mesh-free approximation, the motion and displacements are given by 𝐱(𝜉 , 𝜂, 𝜁 ) = 𝐱̅(𝜉 , 𝜂) + 𝐕(𝜉 , 𝜂, 𝜁 ) ≈ ∑ Ψ̃𝐼(𝜉 , 𝜂)𝐱𝐼 𝑁𝑃 𝑁𝑃 + ∑ Ψ̃𝐼(𝜉 , 𝜂) 𝐼=1 𝐼=1 𝜁 ℎ𝐼 𝐕3𝐼, (43.50) Initial configuration V3 X¯ u¯ V3 x¯ Deformed Configuration Figure 43.5. Deformation of a shell. Element-Free Galerkin LS-DYNA Theory Manual 𝐮(𝜉 , 𝜂, 𝜁 ) = 𝐮̅̅̅̅(𝜉 , 𝜂) + 𝐔(𝜉 , 𝜂, 𝜁 ) ≈ ∑ Ψ̃𝐼(𝜉 , 𝜂)𝐮𝐼 𝑁𝑃 𝑁𝑃 + ∑ Ψ̃𝐼(𝜉 , 𝜂) 𝐼=1 𝐼=1 𝜁 ℎ𝐼 [−𝐕2𝐼 𝐕1𝐼] { 𝛼𝐼 𝛽𝐼 } ,(43.51) where 𝐱𝐼 and 𝐮𝐼 are the global coordinates and displacements at mesh-free node 𝐼, respectively. 𝐕3𝐼 is the unit vector of the fiber director and 𝐕1𝐼, 𝐕2𝐼 are the base vectors of the nodal coordinate system at node 𝐼. 𝛼𝐼 and 𝛽𝐼 are the rotations of the director vector 𝐕3𝐼 about the 𝐕1𝐼 and 𝐕2𝐼 axes. ℎ𝐼 is the thickness. The variables with a superscripted bar refer to the shell mid-surface. Ψ̃𝐼 is the 2D mesh-free shape functions constructed based on one of the two mesh-free surface representations described in the previous section, with (𝜉 , 𝜂) either the parametric coordinates or local coordinates of the evaluated point. The local co-rotational coordinate system (𝑥̂, 𝑦̂, 𝑧̂) is defined at each integration point on the shell reference surface, with 𝑥̂ and 𝑦̂ tangent to the reference surface and 𝑧̂ in the thickness direction . The base vectors are given as 𝐞̂1 = 𝐱,ξ ∥𝐱,ξ∥ , 𝐞̂3 = 𝐱,ξ × 𝐱,η ∥𝐱,ξ × 𝐱,η∥ , 𝐞̂2 = 𝐞̂3 × 𝐞̂1. (43.52) In order to describe the fiber rotations of a mesh-free node in a shell, we introduce a nodal coordinate system whose three base vectors are 𝐕1, 𝐕2 and 𝐕3, see Figure 43.6, where 𝐕3 is the fiber director at the node and 𝐕1, 𝐕2 are defined as follows 𝐕1 = 𝐱̂ × 𝐕3 ∣𝐱̂ × 𝐕3∣ , 𝐕2 = 𝐕3 × 𝐕1. (43.53) The rotation of the fiber director is then obtained from the global rotations: 𝛽} = [ { 𝐕1 T] Δθ, 𝐕2 Δθ = [Δ𝜃1 Δ𝜃2 Δ𝜃3]T. (43.54) LS-DYNA Theory Manual Element-Free Galerkin V3 V2 z^ y^ zs^ ys^ xs^ x^ V1 Figure 43.6. Local co-rotational and nodal coordinate systems. In the local co-rotational coordinate system, the motion and displacements are approximated by the mesh-free shape functions NP x̂i = ∑ Ψ̃Ix̂iI I=1 NP + ζ ∑ Ψ̃I I=1 hI 𝑉̂3𝑖𝐼 , NP ûi = ∑ Ψ̃IûiI I=1 NP + ζ ∑ Ψ̃I I=1 hI [−V̂2iI V̂1iI] { αI βI . } The Lagrangian smoothed strains [Chen et al. 2001b] are given by ε̃m = ∑ 𝐁̃I m𝐝̂ , ε̃b = ζ ∑ 𝐁̃I b𝐝̂ , ε̃s = ∑ 𝐁̃I s𝐝̂ , (43.55) (43.56) (43.57) where the smoothed strain operators are calculated by averaging the consistent strain operators over an area around the evaluated point m(𝐱𝑙) = 𝐁̃𝐼 𝐴𝑙 m𝑑𝐴 ∫ 𝐁̂𝐼 Ω𝑙 , 𝐁̃𝐼 b(𝐱𝑙) = 𝐴𝑙 b𝑑𝐴 ∫ 𝐁̂𝐼 Ω𝑙 , 𝐁̃𝐼 s(𝐱𝐿) = 𝐴𝐿 ∫ 𝐁̂𝐼 Ω𝐿 s𝑑𝐴 , (43.58) with 𝐁̂𝐼 = ⎡Ψ̃𝐼,𝑥 ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎣ 0 −𝐽13 −1Ψ̃𝐼 Ψ̃𝐼,𝑦 0 −𝐽23 −1Ψ̃𝐼 Ψ̃𝐼,𝑦 Ψ̃𝐼,𝑥 0 −𝐽23 −1Ψ̃𝐼 ℎ𝐼 ℎ𝐼 ℎ𝐼 𝑉̂2𝑥𝐼 𝑉̂2𝑦𝐼 −1Ψ̃𝐼 𝐽13 −1Ψ̃𝐼 𝐽23 𝑉̂2𝑥𝐼 − 𝐽13 −1Ψ̃𝐼 ℎ𝐼 𝑉̂2𝑦𝐼 −1Ψ̃𝐼 𝐽23 ℎ𝐼 ℎ𝐼 ℎ𝐼 𝑉̂1𝑥𝐼 𝑉̂1𝑦𝐼 𝑉̂1𝑥𝐼 + 𝐽13 −1Ψ̃𝐼 ⎤ ⎥ ⎥ ⎥ ⎥ ⎥ ⎥ 𝑉̂1𝑦𝐼⎦ ℎ𝐼 , (43.59) Element-Free Galerkin LS-DYNA Theory Manual xl xL Figure 43.7. Integration scheme for mesh-free shells. 𝐁̂𝐼 b = ⎡0 ⎢ ⎢ ⎢ ⎢ ⎢ ⎢ ⎣ 0 −Ψ̃𝐼,𝑥 0 −Ψ̃𝐼,𝑦 0 −Ψ̃𝐼,𝑦 ℎ𝐼 ℎ𝐼 ℎ𝐼 𝑉̂2𝑥𝐼 𝑉̂2𝑦𝐼 Ψ̃𝐼,𝑥 Ψ̃𝐼,𝑦 𝑉̂2𝑥𝐼 − Ψ̃𝐼,𝑥 ℎ𝐼 𝑉̂2𝑦𝐼 Ψ̃𝐼,𝑦 ℎ𝐼 ℎ𝐼 ℎ𝐼 𝑉̂1𝑥𝐼 𝑉̂1𝑦𝐼 𝑉̂1𝑥𝐼 + Ψ̃𝐼,𝑥 ⎤ ⎥ ⎥ ⎥ , ⎥ ⎥ ⎥ 𝑉̂1𝑦𝐼⎦ ℎ𝐼 (43.60) 𝐁̂𝐼 s = −1Ψ̃𝐼 ⎡0 ⎢⎢⎢ ⎣ 𝑉̂2𝑦𝐼 − 𝐽23 0 Ψ̃𝐼,𝑦 −𝐽33 ℎ𝐼 ℎ𝐼 and 𝐉−1 is the inverse of the Jacobian matrix at the integration point. The local degrees- of-freedom are ⎤ ⎥⎥⎥ , (43.61) 𝑉̂1𝑧𝐼⎦ 0 Ψ̃𝐼,𝑥 −𝐽33 𝑉̂1𝑦𝐼 + 𝐽23 𝑉̂1𝑥𝐼 + 𝐽13 𝑉̂2𝑥𝐼 − 𝐽13 ℎ𝐼 ℎ𝐼 ℎ𝐼 ℎ𝐼 ℎ𝐼 ℎ𝐼 −1Ψ̃𝐼 𝐽33 −1Ψ̃𝐼 𝐽33 −1Ψ̃𝐼 −1Ψ̃𝐼 −1Ψ̃𝐼 −1Ψ̃𝐼 −1Ψ̃𝐼 𝑉̂2𝑧𝐼 𝑉̂1𝑧𝐼 𝑉̂2𝑧𝐼 The internal nodal force vector is 𝐝̂ 𝐼 = [𝑢̂𝑥𝐼 𝑢̂𝑦𝐼 𝑢̂𝑧𝐼 𝛼𝐼 𝛽𝐼]T. int = ∫ 𝐁̃I 𝐅̂I mT σ̂ dΩ + ∫ ζ𝐁̃I bT σ̂ sT dΩ + ∫ 𝐁̃I σ̂ dΩ. (43.62) (43.63) The above integrals are calculated with the local boundary integration method. Each background finite element is divided into four integration zones, shown as Ω𝑙 in Figure 43.7. In order to avoid shear locking in the analysis of thin shells, the shear term (third term in Eq. (43.63)), should be under-integrated by using one integration zone in each background element (Ω𝐿 in Figure 43.7). Accordingly, the co-rotational coordinate systems are defined separately at the center of each integration zone, as shown in Figure 43.6. The use of the updated Lagrangian formulation implies that the reference coordinate system is defined by the co-rotational system in the configuration at time t. LS-DYNA Theory Manual Element-Free Galerkin Therefore, the local nodal force and displacement vectors referred to this coordinate system must be transformed to the global coordinate system prior to assemblage. LS-DYNA Theory Manual Linear shells 44 Linear shells 44.1 Shells for Linear Analysis It is common to construct elements for linear analysis by the superimposition of a plate and a membrane element. If the base plates and membrane elements involve only three translational degrees-of-freedom and two in-plane rotational degrees-of-freedom, the resulting element then contains 5 degrees-of-freedom per node since there is an unconstrained rotational degree-of-freedom normal to the mid surface of the shell. This unconstrained mode can cause problems when linking the shell to other elements such as beam elements in three-dimensional space. For this reason, the linear elements in LS- DYNA are based on published formulations that include a drilling degree-of-freedom, which is added to the membrane part of the element to form a 24 degree-of-freedom shell element. These elements pass all patch tests, have 6 rigid body modes, and have no spurious mechanisms. 44.2 Wilson’s Shell (element #20) This quadrilateral element is constructed as described above and is discussed in more detail by Wilson [2000]. The triangular element, which is an 18 degree-of-freedom complement to the quadrilateral elements, follows the same procedure. In a linear analysis in LS-DYNA, automatic sorting is invoked if a mesh has both quadrilateral and triangular elements within a single part ID. This sorting ensures the proper treatment of triangles. 44.2.1 Plate Element The 4 node quadrilateral plate element is based on the 8 node, quadratic quadrilateral plate element, which has 16 rotational degrees-of-freedom, i.e., two per Linear shells LS-DYNA Theory Manual Plate Membrane Figure 44.1. Shell as assembly of plate and membrane elements nodal point. The implementation in LS-DYNA directly follows the textbook by Wilson [2000] where the complete details of the element are provided. A condensed overview is given here. The shell theory makes the following assumptions: •The fiber remains straight and inextensible •The normal stress in the thickness direction is zero The local x and y rotations of the shell are interpolated from the equations: 𝜃𝑥(𝑟, 𝑠) = ∑ 𝑁𝑖 (𝑟, 𝑠)𝜃𝑥𝑖 + ∑ 𝑁𝑖 (𝑟, 𝑠)Δ𝜃𝑥𝑖 𝑖=1 𝑖=5 𝜃𝑦(𝑟, 𝑠) = ∑ 𝑁𝑖 (𝑟, 𝑠)𝜃𝑦𝑖 + ∑ 𝑁𝑖 (𝑟, 𝑠)Δ𝜃𝑦𝑖, 𝑖=1 𝑖=5 (44.1) where nodes 5-8 are at the mid side of the element. The interpolation functions are given by 𝑁1 = 𝑁2 = 𝑁3 = 𝑁4 = (1 − 𝑟)(1 − 𝑠) 𝑁5 = (1 + 𝑟)(1 − 𝑠) 𝑁6 = (1 + 𝑟)(1 + 𝑠) 𝑁7 = (1 − 𝑟)(1 + 𝑠) 𝑁8 = (1 − 𝑟2)(1 − 𝑠) (1 + 𝑟)(1 − 𝑠2) (1 − 𝑟2)(1 + 𝑠) (1 − 𝑟)(1 − 𝑠2). (44.2) In his formulation, Wilson resolves the rotation of the mid side node into tangential and normal components relative to the shell edges. The tangential component is set to zero leaving the normal component as the unknown, which reduces the rotational degrees- of-freedom from 16 to 12, see Figure 44.2. Δ𝜃𝑥 = sin𝛼𝑖𝑗Δ𝜃𝑖𝑗 Δ𝜃𝑦 = −cos𝛼𝑖𝑗Δ𝜃𝑖𝑗 (44.3) LS-DYNA Theory Manual Linear shells ΔΘ ΔΘ ΔΘ ij ij i = 1, 2, 3, 4 j = 2, 3, 4, 1 m =5, 6, 7, 8 Figure 44.2. Element edge [Wilson, 2000] 𝜃𝑥(𝑟, 𝑠) = ∑ 𝑁𝑖 (𝑟, 𝑠)𝜃𝑥𝑖 + ∑ 𝑀𝑥𝑖 (𝑟, 𝑠)Δ𝜃𝑖 𝑖=1 𝑖=5 𝜃𝑦(𝑟, 𝑠) = ∑ 𝑁𝑖 (𝑟, 𝑠)𝜃𝑦𝑖 + ∑ 𝑀𝑦𝑖 (𝑟, 𝑠)Δ𝜃𝑖. 𝑖=1 𝑖=5 (44.4) Ultimately, the 4 mid side rotations are eliminated by using static condensation, a procedure that makes this shell very costly if used in explicit calculations. The local 𝑥 and 𝑦 displacements relative to the mid surface are functions of the 𝑧- coordinate and rotations: 𝑢𝑥(𝑟, 𝑠) = 𝑧𝜃𝑦(𝑟, 𝑠) 𝑢𝑦(𝑟, 𝑠) = −𝑧𝜃𝑥(𝑟, 𝑠). (44.5) Wilson shows, where it is assumed that the normal displacement along each side is cubic, that the transverse shear strain along each side is given by, 𝛾𝑖𝑗 = (𝑢𝑧𝑗 − 𝑢𝑧𝑖) − (𝜃𝑖 + 𝜃𝑗) − Δ𝜃𝑖𝑗, which can be rewritten, referring to Figure 44.3 as: 𝛾𝑖𝑗 = (𝑢𝑧𝑗 − 𝑢𝑧𝑖) − sin𝛼𝑖𝑗 (𝜃𝑥𝑖 + 𝜃𝑥𝑗) + cos𝛼𝑖𝑗 (𝜃𝑦𝑖 + 𝜃𝑦𝑗) − Δ𝜃𝑖𝑗, The nodal shears are then written in terms of the side shears as sin𝛼𝑖𝑗 sin𝛼𝑘𝑖 which can be inverted to obtain the nodal shears: cos𝛼𝑖𝑗 cos𝛼𝑘𝑖 𝛾𝑖𝑗 𝛾𝑘𝑖 ] = [ [ ] [ 𝛾𝑥𝑧 𝛾𝑦𝑧 ], (44.6) (44.7) (44.8) Linear shells LS-DYNA Theory Manual ki ΔΘ ki ki ij ΔΘ ij ij i = 1, 2, 3, 4 j = 2, 3, 4, 1 m =5, 6, 7, 8 xz yz Figure 44.3. Nodal and edge shear strains [Wilson 2000]. 𝛾𝑥𝑧 𝛾𝑦𝑧 [ ] = cos𝛼𝑖𝑗sin𝛼𝑘𝑖 − cos𝛼𝑘𝑖sin𝛼𝑖𝑗 [ sin𝛼𝑘𝑖 −sin𝛼𝑖𝑗 −cos𝛼𝑘𝑖 cos𝛼𝑖𝑗 ] [ 𝛾𝑖𝑗 𝛾𝑘𝑖 ]. (44.9) The standard bilinear basis functions are used to interpolate the nodal shears to the integration points. 44.2.2 Membrane Element The membrane element, which is also coded from Wilson’s textbook [2000], is based on the eight node isoparametric element, see Figure 44.4. The inplane displacement field for the 8 node membrane is interpolated, using the serendipity shape functions with the mid-side relative displacements, from: 𝑢𝑥(𝑟, 𝑠) = ∑ 𝑁𝑖 (𝑟, 𝑠)𝑢𝑥𝑖 + ∑ 𝑁𝑖 (𝑟, 𝑠)Δ𝑢𝑥𝑖 𝑖=1 𝑖=5 𝑢𝑦(𝑟, 𝑠) = ∑ 𝑁𝑖 (𝑟, 𝑠)𝑢𝑦𝑖 + ∑ 𝑁𝑖 (𝑟, 𝑠)Δ𝑢𝑦𝑖. 𝑖=1 𝑖=5 (44.10) It is desired to replace the mid side relative displacment by drilling rotations at the corner nodes. Consider Figure 44.5: the mid-side normal displacements along the edge are parabolic, i.e., Δ𝑢𝑖𝑗 = 𝐿𝑖𝑗 (Δ𝜃𝑗 − Δ𝜃𝑖), (44.11) LS-DYNA Theory Manual Linear shells while the mid-side tangential displacements are interpolated linearly from the end node displacements, thus, Δ𝑢𝑥(𝑟, 𝑠) = cos𝛼𝑖𝑗Δ𝑢𝑖𝑗 = cos𝛼𝑖𝑗 𝐿𝑖𝑗 Δ𝑢𝑦(𝑟, 𝑠) = −sin𝛼𝑖𝑗Δ𝑢𝑖𝑗 = −sin𝛼𝑖𝑗 (Δ𝜃𝑗 − Δ𝜃𝑖) 𝐿𝑖𝑗 (Δ𝜃𝑗 − Δ𝜃𝑖), 𝑢𝑥(𝑟, 𝑠) = ∑ 𝑁𝑖 (𝑟, 𝑠)𝑢𝑥𝑖 + ∑ 𝑀𝑥𝑖 (𝑟, 𝑠)Δ𝜃𝑖 𝑖=1 𝑖=5 𝑢𝑦(𝑟, 𝑠) = ∑ 𝑁𝑖 (𝑟, 𝑠)𝑢𝑦𝑖 + ∑ 𝑀𝑦𝑖 (𝑟, 𝑠)Δ𝜃𝑖. 𝑖=1 𝑖=5 (44.12) (44.13) This element has one singularity in the drilling mode of equal corner rotations, see Figure 44.6. Ibrahimbegovic and Wilson [1991] added a penalty formulation to the potential energy of the element to eliminate the singularity. The following penalty term connects the averaged nodal rotation to the continuum mechanics rotation ( ∂𝑢𝑥 ∂𝑦 − ∂𝑢𝑦 ∂𝑥 ) − 𝜔 (44.14) Figure 44.4. Eight node membrane element. Linear shells LS-DYNA Theory Manual Δuy ΔΘ Δux i = 1, 2, 3, 4 j = 2, 3, 4, 1 m = 5, 6, 7, 8 Δuij ij Lij ΔΘ Figure 44.5. Corner node drilling rotations and mid side edge normal displacement [Wilson, 2000]. Figure 44.6. Zero energy mode at the center of the element. The element performance is highly insensitive to the chosen value of the penalty factor and some fraction of the elastic modulii, G or E, is frequently used. • 5, 8 or 9 point quadrature can be applied. The 5 and 8 point schemes induce a ‘soft’ first deformational mode, whereas the 9 point Gaussian quadrature results in a stiffer mode. • A membrane locking correction (Taylor) is applied to (i) alleviate a membrane- bending interaction associated with the drilling degrees of freedom and (ii) allow LS-DYNA Theory Manual Linear shells the standard application of the consistent nodal load at the edge. The correction has a slight stiffening effect . • A warping correction is applied using the rigid link correction . 44.3 Assumed Strain/Membrane with Drilling Degree-of- freedom (element #18) 44.3.1 Membrane Element Formulation is the same as above for element type 20. 44.3.2 Plate Element The Discrete Kirchhoff Quadrilateral element is an excellent thin shell element based on • Rotational field is interpolated using the 8-node isoparametric parent element. • Transverse displacement w assumed as cubic along the sides and collocated along the sides and at the nodes using the Kirchhoff condition that equates the fiber rotation to the slope. The Kirchhoff assumptions are satisfied along the entire boundary of the element. • The rotational field about an axis parallel to the side is constrained linearly along the sides. The warping correction is applied as above. Flat Element Figure 44.7. Flat element Linear shells LS-DYNA Theory Manual 44.4 Differences between Element Types 18 and 20. The DKQ does not account for transverse shear because it locally enforces the Kirchhoff condition. Hence, element type 20 is better for layered composites and thick plates. LS-DYNA Theory Manual Random Geometrical Imperfections 45 Random Geometrical Imperfections 45.1 Introduction to Random Geometrical Imperfections Using Karhunen-Loève Expansions through using Karhunen-Loève expansions There are different methods of incorporating imperfections, depending on the availability of accurate imperfection data. The method implemented into LS-DYNA v971 uses a spectral decomposition of geometrical or thickness uncertainty, more . To specify the covariance of the random field of the geometrical imperfections or thickness variation, two methods are available. The first is to use available experimentally-measured imperfection fields as input for a principal component analysis based on pattern (face) recognition literature. This method reduces the cost of the resulting eigen-analysis. The second is to specify the covariance function analytically and to solve the resulting Friedholm integral equation of the second kind using a wavelet-Galerkin approach, also obtained from literature. Six different analytical covariance kernels (e.g., exponential and triangular) are available for selection. 45.2 Methodology 45.2.1 Generation of random fields using Karhunen-Loève expansion The Karhunen-Loève expansion (e.g., Ghanem and Spanos [2003]) provides an attractive way of representing a random (stochastic) field (process) through a spectral decomposition, ϖ, as a function of x (e.g., two spatial variables): ∞ 𝜛(x, 𝜃) = 𝜛̅(x) + ∑ √𝜆i𝜉𝑖(𝜃)𝑓𝑖(x) , 𝑖=1 (45.1) where the 𝜉𝑖 are uncorrelated zero-mean random variables with unit variance, and 𝜛̅(x)is the average random field or mean of the process. The functions 𝑓𝑖 are the Random Geometrical Imperfections LS-DYNA Theory Manual eigenfunctions of the covariance kernel, C, with 𝜆𝑖 the associated eigenvalues, obtained from the spectral decomposition of the covariance function via the solution on a domain 𝐷 of the Fredholm integral equation of the second kind, ∫ 𝐶(x1, x2)𝑓𝑖(x1)𝑑x1 = 𝜆𝑖𝑓𝑖(x2). The eigenfunctions form an orthogonal set ∫ 𝑓𝑖(x)𝑓𝑗(x)𝑑x = 𝛿𝑖𝑗. Normally, a finite 𝑀 number of terms are kept in the series expansion: 𝜛(x, 𝜃) = 𝜛̅(x) + ∑ √𝜆i𝜉𝑖(𝜃)𝑓𝑖(x) . (45.2) (45.3) (45.4) 𝑖=1 If 𝜛 is Gaussian, then 𝜉𝑖 are also Gaussian. For non-Gaussian processes (with arbitrary but specified marginal distributions), 𝜉𝑖 are unknown. Phoon et al ([2002a], [2005]) give an iterative procedure for obtaining 𝜉𝑖 given a target marginal distribution. 45.2.2 Solution of Fredholm integral of the second kind for analytical covariance functions The Wavelet-Galerkin method (Phoon et al [2002]) is used to perform the solution, and can be described as follows. By defining a set of basis functions: 𝜑1(𝑥), 𝜑2(𝑥),…,𝜑𝑁(𝑥), each eigenfunction 𝑓𝑖(𝑥) can be approximated by the linear combination: 𝑓𝑖(𝑥) = ∑ 𝑑𝑖𝑘 𝜑𝑘(𝑥), 𝑘=1 (45.5) where the 𝑑𝑖𝑘 are constant coefficients. By substituting (45.5) into Fredholm equation (45.2) (using a scalar 𝑥 (one-dimensional random process) as an example) and writing as an error: ∫ 𝐶(x1, x2) ∑ 𝑑𝑖𝑘𝜑𝑘(𝑥1)𝑑x1 𝑘=1 − 𝜆𝑖 ∑ 𝑑𝑖𝑘𝜑𝑘(𝑥1) = 0. 𝑘=1 (45.6) By making the error orthogonal to the basis functions: ⎢⎡∫ 𝐶(x1, x2) ∑ 𝑑𝑖𝑘𝜑𝑘(𝑥1)𝑑x1 ⎣ 𝑘=1 ⎥⎤ − 𝜆𝑖 ∑ 𝑑𝑖𝑘𝜑𝑘(𝑥1) ⎦ 𝑘=1 𝜑𝑗(𝑥2)𝑑𝑥2 = 0, (45.7) ∫ we get ∑ 𝑑𝑖𝑘 𝑘=1 ⎢⎡∬ 𝐶(x1, x2) ⎣ 𝜑𝑘(𝑥1)𝜑𝑗(𝑥2)𝑑x1𝑑x2 ⎥⎤ − 𝜆𝑖 ∑ 𝑑𝑖𝑘 ⎦ 𝑘=1 ⎢⎡∫ 𝜑𝑘(𝑥2)𝜑𝑗(𝑥2)𝑑x2 ⎣ ⎥⎤ ⎦ = 0, (45.8) LS-DYNA Theory Manual Random Geometrical Imperfections or the eigensystem 𝐀𝐃 = 𝚲𝐁𝐃 with Λ𝑖𝑗 = 𝛿𝑖𝑗𝜆𝑗. Orthogonal wavelets 𝜓(𝑥) are used (∫ 𝜓𝑗(x)𝜓𝑘(x)𝑑x functions, 𝐟𝑖(𝑥) = ∑ 𝑑𝑖𝑘 𝑘=1 𝜓𝑘(𝑥) = 𝛙T(𝑥)𝐃(𝑖), so that the covariance function can be expressed as: (45.9) = ℎ𝑗𝛿𝑗𝑘) as basis (45.10) 𝐶(𝐱1, 𝐱2) = ∑ ∑ 𝐴̅𝑗𝑘𝜓𝑗(𝐱1)𝜓𝑘(𝐱2) = 𝛙T(𝐱1)𝐀̅̅̅̅̅̅ 𝛙(𝐱2), (45.11) 𝑗=1 where 𝐀̅̅̅̅̅̅ is the 2D wavelet transform of 𝐶(𝐱1, 𝐱2) given by 𝑘=1 𝐴̅𝑗𝑘 = ℎ𝑗ℎ𝑘 ∫ ∫ 𝐶(𝐱1, 𝐱2)𝜓𝑗(𝐱1)𝜓𝑘(𝑥2)𝑑x1𝑑x2 . Substituting (45.10) and (45.11) into (45.2), we again get an eigenvalue problem 𝛙T(𝑥)𝐀̅̅̅̅̅̅𝐇𝐃(𝑖) = 𝜆𝑖𝛙T(𝑥)𝐃(𝑖). (45.12) (45.13) 2⁄ 𝐃(𝑖) and 𝐀̂ = Or, equating coefficients of 𝛙T and using the transformation 𝐃̂ (𝑖) = 𝐇 2⁄ , the eigensystem 2⁄ 𝐀̅̅̅̅̅̅𝐇 The eigenvectors from (45.14) are transformed to the eigen functions (of (45.9)) by the equation: 𝐀̂𝐃̂ (𝑖) = 𝜆𝑖𝐃̂ (𝑖). (45.14) 𝐟𝑖(𝑥) = 𝛙T(𝑥)𝐇−1 2⁄ 𝐃̂ (𝑖). (45.15) The double integral in (45.12) is constructed using two successive 1D discrete wavelet transforms in the form of Mallat’s tree algorithm (Phoon et al [2002a]). Haar wavelets are used because of their simplicity and ability to capture the field characteristics. The eigenfunctions (45.15) and associated eigenvalues 𝜆𝑖 can be used to construct random fields (using (45.4)) with the same second-order statistics as the covariance model used. The available covariance functions (Ghanem and Spanos [2003]), are: • Exponential covariance function (First-order Markov process (autoregressive)), 𝐶(x1, x2) = exp ( −|𝑥1 − 𝑥2| 𝐿𝑐 ) (45.16) • Triangular covariance function Random Geometrical Imperfections LS-DYNA Theory Manual 𝐶(x1, x2) = 1 − |𝑥1 − 𝑥2| 𝐿𝑐 • Sine covariance function 𝐶(x1, x2) = sin𝐿𝑐(𝑥1 − 𝑥2) 𝐿𝑐(𝑥1 − 𝑥2) • Squared exponential covariance function 𝐶(x1, x2) = exp ( −|𝑥1 − 𝑥2|2 𝐿𝑐 ) • Wiener-Levy covariance function 𝐶(x1, x2) = min(x1, x2) • Uniformly modulated nonstationary covariance function 𝐶(x1, x2) = exp(−(𝑥1 − 𝑥2))exp −|𝑥1 − 𝑥2| 𝐿𝑐 with 𝐿𝑐 the correlation length in the respective direction. (45.17) (45.18) (45.19) (45.20) (45.21) 45.2.3 Generating eigenfunctions from experimentally measured fields If experimentally measured random fields are available, then the eigenfunctions and eigenvalues in (45.1) or (45.4) can be determined from the second-order statistics of the measurements. Following the pattern recognition method proposed by Turk and Pentland [1991], the procedure described next is used. Given a set of 𝑀 field measurements, e.g., geometrical imperfections on an 𝑁1 × 𝑁2 mesh, we can represent the measurements as 1-D vectors of length 𝑁1 × 𝑁2, i.e., Γ1, …, Γ𝑀. The average vector is defined by 𝚿 = ∑ 𝚪𝑛 𝑛=1 , (45.22) allowing us to define the deviation of each measured field from the average, also as a vector: 𝚽𝑖 = 𝚪𝑖 − 𝚿. Combining the deviation vectors into a covariance matrix, 𝐂, we get 𝐂 = ∑ 𝚽𝑛𝚽𝑛 𝑛=1 = 𝐀𝐀T, (45.23) where 𝐀 = [𝚽1 𝚽2 … 𝚽𝑀]. The covariance matrix has a set of orthonormal eigenvectors, 𝐟𝑖, and associated eigenvalues, 𝜆𝑖 obtained through a principal component analysis, i.e., LS-DYNA Theory Manual Random Geometrical Imperfections The eigenpairs are chosen such that 𝐀𝐀T𝐟𝑖 = 𝜆𝑖𝐟𝑖. is a maximum, subject to 𝜆𝑖 = ∑(𝐟𝑖 𝑛=1 T𝚽𝑛) , T𝐟𝑘 = 𝛿𝑙𝑘, 𝐟𝑖 (45.24) (45.25) (45.26) with 𝛿 the Kronecker delta. As the size of the covariance matrix is (𝑁1 × 𝑁2)2, determining the eigenvectors and eigenvalues in (41.24) can be a time-consuming and memory-intensive task for large measurement meshes. This computation can be simplified if the number of measurement samples is less than the mesh count (𝑀 < 𝑁1 × 𝑁2), as there are then only 𝑀– 1, rather than 𝑁1 × 𝑁2, meaningful eigenvectors. This is done by considering the eigenvectors of another matrix 𝐋 = 𝐀T𝐀, as embodied in the eigensystem 𝐀T𝐀v𝑖 = 𝜇𝑖𝐯𝑖. Premultiplying both sides in (20.1.6) by 𝐀, we get 𝐀𝐀T𝐀𝐯𝑖 = 𝜇𝑖𝐀𝐯𝑖, (45.27) (45.28) which implies that the 𝑀 – 1 eigenvectors, 𝐀𝐯𝑖, are also eigenvectors of 𝐀𝐀Tor 𝐂. The 𝑇 𝚽𝑛. eigensystem in (20.1.6), however, is only size (𝑀 × 𝑀), as 𝐋 = 𝐀T𝐀, where 𝐿𝑛𝑚 = 𝚽𝑚 Once the eigenvectors of 𝐋 are obtained, the required eigenfunctions, 𝐟𝑖, are recovered through the linear combination 𝐟𝑖 = ∑ v𝑖𝑘𝚽𝑘 𝑘=1 , 𝑖 = 1, … , 𝑀 (45.29) The 𝑀 – 1 eigenvalues of 𝐋 and 𝐂 are identical, i.e., 𝜆𝑖 = 𝜇𝑖. Finally 𝐟𝑖and 𝜆𝑖 are used in (45.4) to construct the required Karhunen-Loève expansion of the random fields. LS-DYNA Theory Manual Frequency Domain 46 Frequency Domain 46.1 Frequency Response Functions Frequency response function (FRF) is a characteristic of a system that has a measured or computed response resulting from a known applied input. Mathematical- ly it is a transfer function and expresses the structural response to an applied force as a function of frequency. The response can be given in terms of displacement, velocity, or acceleration. Frequency response functions are complex functions, with real and imaginary components. They can also be written in terms of magnitude and phase pairs. 46.1.1 FRF Computations FRF is computed using mode superposition method, in frequency domain. When damping is included, the dynamic response of a system is governed by 𝐦𝐮̈ + 𝐜𝐮̇ + 𝐤𝐮 = 𝐩(𝑡), (46.1.1) where 𝐦, 𝐜 and 𝐤 are the mass, damping and stiffness matrices, 𝐩(𝑡) is the external force. Using the mode superposition method, the displacement response can be expressed by 𝐮 = ∑ 𝜙𝑛𝑞𝑛(𝑡) = Φq, (46.1.2) 𝑛=1 where 𝜙𝑛 is the n-th mode shape and 𝑞𝑛(𝑡) is the n-th modal coordinates. With the substitution of Equation (46.1.2) into Equation (46.1.1), the governing equation can be rewritten as Pre-multiplying by ΦT gives 𝐦𝚽𝐪̈ + 𝐜𝚽𝐪̇ + 𝐤𝚽𝐪 = 𝐩(𝑡). 𝐌𝐪̈ + 𝐂𝐪̇ + 𝐊𝐪 = 𝐩(𝑡), (46.1.3) (46.1.4) Frequency Domain LS-DYNA Theory Manual The orthogonality of natural modes implies that the following square matrices are diagonal: where the diagonal elements are 𝐌 ≡ 𝚽𝐓𝐦𝚽, 𝐊 ≡ 𝚽𝐓𝐤𝚽, 𝐌𝒏 = 𝛟𝒏 𝐓𝐦𝛟𝒏, 𝐊𝒏 = 𝛟𝒏 𝐓𝐤𝛟𝒏 (46.1.5) (46.1.6) Since 𝐦 and 𝐤 are positive definite, the diagonal elements of 𝐌 and 𝐊 are positive. They are related by The square matrix 𝐂 is obtained similarly as follows 𝐊𝒏 = 𝛚𝒏 𝟐𝐌𝒏. 𝐂 = 𝚽𝐓𝐜𝚽. (46.1.7) (46.1.8) 𝐂 may or may not be diagonal, depending on the distribution of damping in the system. If 𝐂 is diagonal (the diagonal elements are 𝐶𝑛 = 𝜙𝑛 represents N uncoupled differential equations in modal coordinates 𝑞𝑛, and the system is said to have classical damping and the systems possess the same natural modes as those of the undamped system. Only the classical damping is considered in this approach. 𝑇𝑐𝜙𝑛), Equation (46.1.4) The right hand side vector (generalized force) 𝐏(𝑡) is For an N-DOF system with classical damping, each of the N differential equations in modal coordinates is 𝐏(𝑡) = ΦT𝑝(𝑡) (46.1.9) or, 𝑀𝑛𝑞 ̈𝑛 + 𝐶𝑛𝑞 ̇𝑛 + 𝐾𝑛𝑞𝑛 = 𝑃𝑛(𝑡) where the modal damping coefficient 𝑞 ̈𝑛 + 2𝜁𝑛𝜔𝑛𝑞 ̇𝑛 + 𝜔𝑛 2𝑞𝑛 = 𝑃𝑛(𝑡) 𝑀𝑛 ζ is defined as 𝜁𝑛 = 𝐶𝑛 2𝑀𝑛𝜔𝑛 (46.1.10) (46.1.11) (46.1.12) Applying Fourier transform to both sides of Equation (46.1.11), one obtains (−𝜔2 + 2𝑖𝜁𝑛𝜔𝑛𝜔 + 𝜔𝑛 2)𝑞𝑛(𝜔) = 𝑃𝑛(𝜔) 𝑀𝑛 (46.1.13) The structural displacement response in frequency domain can be represented as 𝐮(𝜔) = ∑ 𝑛=1 𝜙𝑛 2) (−𝜔2 + 2𝑖𝜁𝑛𝜔𝑛𝜔 + 𝜔𝑛 𝑃𝑛(𝜔) 𝑀𝑛 46-2 (Frequency Domain) LS-DYNA Theory Manual Frequency Domain Thus the displacement frequency response function (Compliance) can be expressed as (suppose that the excitation is applied at node j and the response is evaluated for node k) 𝐅𝐑𝐅𝒖(𝑥𝑗, 𝑥𝑘, 𝜔) = ∑ 𝑛=1 𝜙𝑛(𝑥𝑘) 2) (−𝜔2 + 2𝑖𝜁𝑛𝜔𝑛𝜔 + 𝜔𝑛 𝑃̃𝑛(𝑥𝑗) 𝑀𝑛 The velocity frequency response function (Mobility) can be expressed as 𝐅𝐑𝐅𝒗(𝑥𝑗, 𝑥𝑘, 𝜔) = 𝜔𝑖 ∑ 𝑛=1 𝜙𝑛(𝑥𝑘) 2) (−𝜔2 + 2𝑖𝜁𝑛𝜔𝑛𝜔 + 𝜔𝑛 𝑃̃𝑛(𝑥𝑗) 𝑀𝑛 (46.1.15) (46.1.16) The acceleration frequency response function (Accelerance) can be expressed as 𝐅𝐑𝐅𝒂(𝑥𝑗, 𝑥𝑘, 𝜔) = −𝜔2 ∑ 𝑛=1 𝜙𝑛(𝑥𝑘) 2) (−𝜔2 + 2𝑖𝜁𝑛𝜔𝑛𝜔 + 𝜔𝑛 𝑃̃𝑛(𝑥𝑗) 𝑀𝑛 where ~ n xP ( ) is obtained as 𝑃̃𝑛(𝑥𝑗) = 𝜙𝑛 𝑇𝑝̃(𝑥𝑗) (46.1.17) (46.1.18) and (~ jxp force excitation, ) is the space distribution of the harmonic force excitation (in the case of point (~ jxp = 1) at node j in specified direction of excitation and 0 elsewhere). 46.1.2 About the damping Damping can be given in several forms . A very common type of damping used in the nonlinear analysis of structure is to assume that the damping matrix is proportional to the mass and stiffness matrices, or This type of damping is normally referred to as Rayleigh damping. For 𝐜 = 𝛼𝐦 + 𝛽𝐤 (46.1.19) classically damped system, Due to the orthogonality of the mass and stiffness matrices, it can be rewritten as 2𝝎𝒏𝜁𝑛 = 𝜙𝑛 𝑇𝐜𝜙𝑛 (46.1.20) or, 2𝝎𝒏𝜁𝑛 = 𝛼 + 𝛽𝜔𝑛 𝜁𝑛 = 2𝜔𝑛 + 𝜔𝑛 (46.1.21) (46.1.22) Frequency Domain LS-DYNA Theory Manual 46.2 ACOUSTIC FEM A frequency domain acoustic finite element method has been implemented in LS-DYNA, to model the acoustic behavior of a confined acoustic fluid volume. This method is based on nodal velocity/pressure formulation. Three types of elements are available. They are hexahedron, pentahedron, and tetrahedron elements. 46.2.1 Theory basis The governing equation for the acoustic problem is the Helmholtz equation. ∇𝟐𝑝 + 𝑘𝟐𝑝 = 0 (46.2.1) where 𝑝 is the acoustic pressure; 𝑘 = 𝜔/𝑐 is called the wave number; 𝜔 = 2𝜋𝑓 is the circular frequency of the acoustic wave; and 𝑐 is the wave speed. For vibro-acoustic problems, the boundary condition is given as follows, 𝜕𝑝 𝜕𝑛 = −𝑖𝜌𝜔𝑣𝑛 (46.2.2) where 𝑛 is the normal vector pointing outside from the acoustic volume; 𝑖 = √−1 is the imaginary unit; 𝜌 is the acoustic fluid density and 𝑣𝑛 is the normal velocity. Using the weighted residue technique and taking the shape function 𝑁𝑖 as the weighting function, the governing equation can be written as ∫ ∇2𝑝𝑁𝑖𝑑𝑉 + ∫ 𝑘2𝑝𝑁𝑖𝑑𝑉 = 0 Using the Green’s theorem, Equation (2.3) can be written as − ∫ ∇𝑝∇𝑁𝑖𝑑𝑉 + 𝑘2 ∫ 𝑝𝑁𝑖𝑑𝑉 = − ∫ 𝜕𝑝 𝜕𝑛 𝑁𝑖𝑑Γ (46.2.3) (46.2.4) With the substitution of the boundary condition (46.2.2) into Equation (46.2.4), and taking the nodal pressure as the unknown variables, a linear equation system can be established and solved in frequency domain. Since there is only one variable on each node, this method is very fast. LS-DYNA Theory Manual Rotor Dynamics 47 Rotor Dynamics 47.1 Introduction Rotor dynamics is a specialized branch of engineering science concerned with the behavior and diagnosis of rotating structures. It is a study of vibration of rotating parts found in a wide range of equipment including engine, turbine, aircraft, hard disk drive and more. The analysis of the rotator dynamics involves two coordinate systems: rotating and fixed coordinate systems. The equations of motion in the two coordinate systems are both introduced. 47.2 Two Coordinate systems The interpretation of rotational phenomena requires the introduction of a rotating coordinate system in relation to the fixed coordinate system. Figure 1.1 depicts the relationship between the two coordinate systems. OXYZ is the fixed coordinate system and oxyz is the rotating coordinate system. R is the location vector of the disk center; r is the location vector of a point P with respect to the rotating coordinate system. Let the velocity of rotation be defined as (cid:3). Rotor Dynamics LS-DYNA Theory Manual Figure 1.1 A rotating disk in two coordinate systems. The position of the point P with respect to OXYZ is 𝒓 ̅, so 𝒓 ̅ = 𝑹 + 𝒓. The velocity of point P is: 𝒗̅̅̅̅ = 𝑑𝒓 ̅ 𝑑𝑡 = 𝑑𝑹 𝑑𝑡 + 𝑑𝒓 𝑑𝑡 = 𝑽 + 𝒗 + 𝜴 × 𝒓, (47.1) (47.2) where 𝑽 (=𝑑𝑹 coordinate system. 𝑑𝑡 ) is the velocity of the origin o; 𝒗 is the velocity of point P in the rotating The acceleration of point P can be calculated as: 𝒂̅ = 𝑑𝒗̅̅̅̅ 𝑑𝑡 = 𝑑𝑽 𝑑𝑡 + 𝑑𝒗 𝑑𝑡 + 𝑑(𝜴 × 𝒓 ) 𝑑𝑡 = 𝑨 + 𝒂 + 𝟐𝜴 × 𝒗 + 𝜴 × (𝜴 × 𝒓) + 𝒅𝜴 𝑑𝑡 × 𝒓, (47.1) where, 𝑨 is the acceleration of the origin o, 𝒂 is the acceleration of point P in rotating coordinate system. We assume that the origin of the rotating coordinate system is fixed, so that: By substituting (1.4) to (1.3): 𝑽 = 𝑨 = 𝟎 . 𝒂̅ = 𝒂 + 𝟐𝜴 × 𝒗 + 𝜴 × (𝜴 × 𝒓) + 𝑑𝜴 𝑑𝑡 × 𝒓 . (47.2) (47.3) 47.3 Forces in the Rotating Coordinate System We now place a particle with mass m into the position of the point P we were following. From (1.5), we can express the force of the particle in the rotating system as: LS-DYNA Theory Manual Rotor Dynamics 𝑭 = 𝑚𝒂 = 𝑚𝒂̅ − 2𝑚𝜴 × 𝒗 − 𝑚𝜴 × (𝜴 × 𝒓) − 𝑚 𝐝𝛀 𝐝t × 𝐫. (47.4) The first term 𝑚𝒂̅ is the force in the fixed coordinate system. All other terms on the right hand side are inertia forces arising in the rotating system. The Coriolis force is the following quantity: The third term produces the familiar centrifugal force: 𝑭𝑪 = −2𝑚𝜴 × 𝒗. 𝑭𝑪𝒇 = −𝑚𝜴 × (𝜴 × 𝒓). (47.5) (47.6) The last term introduces the Euler fore when there is a nonzero rate of change in the magnitude of the rotation vector: 𝑭𝑬 = −𝑚 𝒅𝜴 𝒅𝑡 × 𝒓. (47.7) 47.4 Transformation between Coordinate Systems Let’s assume that the rotation axis coincides with one of the axis of the rotating coordinate system, specifically to the z axis. An arbitrary rotation axis will be discussed later. In this case, the rotational velocity becomes: 𝜴 = 0 ∙ 𝒊 + 0 ∙ 𝒋 + Ω ∙ 𝒌. (47.8) We further restrict our computations to constant rotational velocity; hence the Euler force will not appear in the formulations (Euler force is easy to add to our equations if the rotational velocity is not constant though). We write the location of a particle in the rotating coordinate system as: 𝒓 = { }. It is transformed to the location in the fixed system as follows: 𝐫 ̅ = {⎧𝑥̅ }⎫ 𝑦̅ 𝑧̅⎭}⎬ ⎩{⎨ = 𝑐𝑜𝑠Ωt −𝑠𝑖𝑛Ωt ⎢⎡ 𝑐𝑜𝑠Ωt 𝑠𝑖𝑛Ωt ⎣ ⎥⎤ { 1⎦ } = 𝑯 { }. (47.9) (47.10) 𝑯 is the transformation matrix. It is easy to get that 𝑯 𝑇𝑯 = 𝑰, where 𝑰 is he identity matrix. Other matrices that may be used later are also given here: 𝑯̇ = Ω −𝑠𝑖𝑛Ωt −𝑐𝑜𝑠Ωt ⎢⎡ 𝑐𝑜𝑠Ωt −𝑠𝑖𝑛Ωt ⎣ ⎥⎤ = Ω𝐇̅̅̅̅̅̅, 0⎦ (47.11) Rotor Dynamics LS-DYNA Theory Manual 𝑯̈ = Ω2 sinΩt −𝑐𝑜𝑠Ωt ⎢⎡ −𝑠𝑖𝑛Ωt −𝑐𝑜𝑠Ωt ⎣ ⎥⎤ = Ω2𝐇̿̿̿̿̿̿, 0⎦ 𝑯̅̅̅̅̅ 𝑇𝑯 = −1 ⎢⎡ ⎣ ⎥⎤ = 𝑷, 0⎦ 𝑯 𝑇𝑯̅̅̅̅̅ = 0 −1 ⎢⎡ ⎣ ⎥⎤ = 𝐏T = −𝑷, 0⎦ 𝑯̅̅̅̅̅ 𝑇𝑯̅̅̅̅̅ 𝑇 = ⎢⎡ ⎣ ⎥⎤ = 𝐉. 0⎦ (47.12) (47.13) (47.14) (47.15) 47.5 Equation of Motion in Rotating Coordinate System When the particle undergoes a nodal translation in the rotating coordinate system as shown in Figure 1.2, it can be defined as: 𝒖 = { }. The location vector in the fixed coordinate is: 𝒓 ̅ = 𝑯(𝒓 + 𝒖) (47.16) (47.17) After calculate the velocity in the fixed coordinate system, we can get the kinetic energy due to translation displacement as: 𝑇 = 𝑚Ω2 (𝒓𝑇𝑱𝒓 + 2𝒓𝑇𝑱𝒖 + 𝒖𝑇𝑱𝒖) + (2Ω𝒖̇𝑇𝑷𝑇𝒓 + 2Ω𝒖𝑇𝑷𝒖̇ + 𝒖̇𝑇𝒖̇). (47.18) Figure 1.2 Translation nodal displacement. LS-DYNA Theory Manual Rotor Dynamics Figure 1.3 Rotational nodal displacement. The nodal displacement of the point can also be rotational as shown in Figure 1.3. We assume small rotation of the rotating point: {⎧𝜑 }⎫ 𝜃⎭}⎬ ⎩{⎨ The nodal rotation requires the consideration of mass and inertia. The center of the mass point is coincident with the node. The inertia moment can be given with the concentrated mass input of commercial finite element codes, or they can be defined in connection with the surrounding mass point, or even with a simplified model by attaching six submasses to the node, as shown in figure 1.4. 𝛉 = (47.19) . Figure 1.4 Node with six masses located at offset x’, y’ and z’ from the node center. With this, the location vector in the fixed coordinate is of the form if only considers rotational displacement: where 𝒓 ̅ = 𝑯(𝒓 + 𝒖) = 𝑯(𝒓 + 𝑨𝛉), 𝑨 = −𝑧′ 𝑦′ −𝑥′ 𝑧′ −𝑦′ ⎤. 𝑥′ ⎥ 0 ⎦ ⎡ ⎢ ⎣ (47.20) (47.21) Then we can get the kinetic energy due to rotational displacement as: 𝑇 = 𝑚Ω2 (𝒓𝑇𝑱𝒓 + 𝟐𝒓𝑇𝑱𝑨𝛉 + 𝛉𝑻 𝑨𝑇𝑱𝑨𝛉) + (2Ω𝒓𝑇𝑷𝑨𝛉̇ + 2Ω𝛉𝑇𝑨𝑇𝑷𝑨𝛉̇ + 𝛉̇𝑇𝑨𝑇𝑨𝛉̇). (47.22) Rotor Dynamics LS-DYNA Theory Manual Applying Lagrange’s equation, then we can obtain the final equation of motion as follows: 𝑪𝒖 𝟎 𝑪𝛉 ] {𝒖̇ 𝑴𝒖 𝟎 𝑴𝛉 ] {𝒖̈ [ 𝛉̈} + 2Ω [ 𝛉̇} − Ω2 [ where 𝑴𝒖 and 𝑴𝛉 are the mass and inertia matrices; 𝑪𝒖 and 𝑪𝛉 are the gyroscopic matrices; 𝒁𝒖 and 𝒁𝛉 are the centrifugal softening matrices; 𝑭𝒄𝒖 and 𝑭𝒄𝛉 are centrifugal force. Note that we don’t consider the other system damping and external force terms here, but they can be added to (1.25) accordingly. } = { (47.23) ] { }, 𝒁𝒖 𝟎 𝒁𝛉 𝑭𝒄𝒖 𝑭𝒄𝛉 47.6 Equation of Motion in Fixed Coordinate System The location vector in the fixed coordinate is: 𝒓 ̅ = 𝑯(𝒓 + 𝒖) = 𝑯𝒓 + 𝒖̅. (47.24) Here the 𝒖̅ represents the displacement of the point in the fixed coordinate system due to the nodal translation displacement. Similar analysis as in section 1.5 can be done for the equation of motion in fixed coordinate system. We only give the final equation here: [ ] {𝒖̇ ] {𝒖̅ 𝛉̅̅̅̅̈} + Ω [ 𝑴𝒖̅ 𝟎 𝑴𝛉̅̅̅̅̅ 0 𝑪𝛉̅̅̅̅̅ where 𝑴𝒖̅ and 𝑴𝛉̅̅̅̅̅ are the mass and inertia matrices; 𝑪𝛉̅̅̅̅̅ is the gyroscopic matrix; 𝑭𝒄𝒖̅ is the centrifugal force. All of them are written in the fixed coordinate system. Note that only nodal rotations contributed to the gyroscopic matrix. Same as before, we don’t consider the other system damping and external force terms here, but they can be added to (1.27) accordingly. 𝛉̇} = { 𝑭𝒄𝒖̅ (47.25) }, 47.7 Arbitrary Rotation Axis All the above analysis is based on the assumption that the rotation axis is coincide with the z-axis. Here we will give a way to transform all variables back to global if the rotation axis is not coincide with the z-axis (Figure 1.5). The transformation matrix from z axis to rotation axis is denoted as T and it is easy to get 𝑻 𝑇𝑻 = 𝑰 . 47-6 (Rotor Dynamics) LS-DYNA Theory Manual Rotor Dynamics Figure 1.5 Rotation axis not coincide with z axis. The location vector in the fixed coordinate becomes: 𝒓 ̅ = 𝑻 𝑇𝑯(𝒓′ + 𝒖′). (47.26) where 𝒓′ and 𝒖′ are the location vector and displacement in the coordinate system Ox’y’z’, in which the z axis is transformed to the rotation axis z’ by rotation matrix 𝑻.At the same time: 𝒓′ = 𝑻𝒓 , 𝒖′ = 𝑻𝒖. (47.27) (47.28) where, 𝒓 and 𝒖 are the location vector and displacement in the rotating coordinate system Oxyz. The equation of motion in (1.25) and (1.27) can be simplified written as: And the force term can be written as 𝑴𝟎𝒂 + 𝑪𝟎𝒗 + 𝑲𝟎𝒖 = 𝑭𝟎, 𝑭𝟎 = 𝒇𝟎𝒓, (47.29) (47.30) By substituting (1.28), (1.29) and (1.30) to the equation of motion, we can get new mass, damping, stiffness matrices and force vector as follows: 𝑴 = 𝑻 𝑻 𝑴𝟎𝑻 , 𝑪 = 𝑻 𝑻 𝑪𝟎𝑻, 𝑲 = 𝑻 𝑻 𝑲𝟎𝑻, 𝑭 = 𝑻 𝑻 𝒇𝟎𝑻𝒓. (47.31) (47.32) (47.33) (47.34) So the equation of motion becomes: Rotor Dynamics LS-DYNA Theory Manual 𝑴𝒂 + 𝑪𝒗 + 𝑲𝒖 = 𝑭 . (47.35) After the equation of motion is obtained, it can then be solved using the implicit solver. Especially, the damping and stiffness matrices are related to the rotational velocity, so the eigen-frequencies might change with the change of rotational velocity. A diagram to represent this relationship is called Campbell diagram. An example is given in Figure 1.6. LS-DYNA Theory Manual Rotor Dynamics Figure 1.6 A disk is spinning with the center axis, the mode frequencies change with the increase of rotating speed. LS-DYNA Theory Manual References 48 References Abbo A.J., S.W. Sloan, “A Smooth Hyperbolic Approximation to the Mohr-Coulomb Yield Criterion,” Computers and Structures, Vol 54, No 1, 1995. Addessio, F.L., D.E. Carroll, J.K. Dukowicz, F.H. Harlow, J.N. Johnson, B.A. Kashiwa, M.E. Maltrud, H.M. Ruppel, “CAVEAT: A Computer Code for Fluid Dynamics Problems with Large Distortion and Internal Slip,” Report LA-10613-MS, UC-32, Los Alamos National Laboratory (1986). Ahmad, S., Irons, B.M. and Zienkiewicz, O.C., “Analysis of Thick and Thin Shell Structures by Curved Finite Elements,” Int. J. Numer. Meths. Eng., 2 (1970). Amsden, A. A., and Hirt, C. W., “YAQUI: An Arbitrary Lagrangian-Eulerian Computer Program for Fluid Flow at All Speeds,” Los Alamos Scientific Laboratory, LA-5100 (1973). Amdsden, A., A., Ruppel, H. M., and Hirt, C. W., “SALE: A Simplified ALE Computer Program for Fluid Flow at All Speeds,” Los Alamos Scientific Laboratory (1980). Argyris, J.H., Kelsey, S., and Kamel, H., “Matrix Methods of Structural Analysis: A Precis of recent Developments,” Matrix Methods of Structural Analysis, Pergamon Press (1964). Arruda, E., and M. Boyce, "A Three-Dimensional Constitutive Model for the Large Stretch Behavior of Rubber Elastic Materials," published in the Journal of the Mechanics and Physics of Solids, Vol. 41, No. 2, 389-412 (1993). Auricchio, F., Taylor, R.L. and Lubliner J., “Shape-memory alloys: macromodelling and numerical simulations of the superelastic behavior”, Computer Methods in Applied Mechanics and Engineering 146, 281-312 (1997). References LS-DYNA Theory Manual Auricchio, F. and Taylor, R.L., “Shape-memory alloys: modeling and numerical simulations of the finite-strain superelastic behavior”, Computer Methods in Applie Mechanics and Engineering 143, 175-194 (1997). Back, S.Y., and Will, K.M., “A Shear-flexible Element with Warping for Thin-Walled Open Sections,” International Journal for Numerical Methods in Engineering, 43, 1173-1191 (1998). Bahler AS: The series elastic element of mammalian skeletal muscle. Am J Physiol 213:1560-1564, 1967. Bammann, D. J., and E.C. Aifantis, “A Model for Finite-Deformation Plasticity,” Acta Mechanica, 70, 1-13 (1987). Bammann, D. J., “Modeling the Temperature and Strain Rate Dependent Large Deformation of Metals,” Proceedings of the 11th US National Congress of Applied Mechanics, Tucson, AZ (1989). Bammann, D. J., and Johnson, G., “On the Kinematics of Finite-Deformation Plasticity,” Acta Mechanica 69, 97-117 (1987). Bammann, D.J., Chiesa, M.L., McDonald, A., Kawahara, W.A., Dike, J.J. and Revelli, V.D., “Predictions of Ductile Failure in Metal Structures,” in AMD-Vol. 107, Failure Criteria and Analysis in Dynamic Response, edited by. H.E. Lindberg, 7-12 (1990). Bandak, F.A., private communications, U.S. Dept. of Trans., Division of Biomechanics Research, 400 7th St., S.W. Washington, DC 20590 (1991). Barlat and Lian, J., “Plastic Behavior and Stretchability of Sheet Metals, Part I: A Yield Function for Orthotropic Sheets Under Plane Stress Conditions,” International Journal of Plasticity, 5, 51-66 (1989). Barlat, F., Lege, D.J., and Brem, J.C., “A Six-Component Yield Function for Anisotropic Materials,” International Journal of Plasticity, 7, 693-712 (1991). Bathe, K. J., Finite Element Procedures in Engineering Analysis, Prentice-Hall (1982). Bathe, K. J., and Wilson, E.L., Numerical Methods in Finite Element Analysis, Prentice- Hall (1976). Bathe, K.J., and Dvorkin, E.N., “A Continuum Mechanics Based Four Node Shell Element for General Nonlinear Analysis,” Int. J. Computer-Aided Eng. and Software, Vol. 1, 77-88 (1984). LS-DYNA Theory Manual References Bathe, K.-J. and Dvorkin, E.N. A four node plate bending element based on Mindlin- Reissner plate theory and a mixed interpolation, Int. J. Num. Meth. Eng., 21, 367-383, 1985. Batoz, J.L. and Ben Tahar, M. Evaluation of a new quadrilateral thin plate bending element, Int. J. Num. Meth. Eng., 18, 1644-1677, 1982. Battini, J., and Pacoste C., “Co-rotational Beam Elements with Warping Effects in Instability Problems,” Computational Methods in Applied Mechanical Engineering, 191, 1755-1789, (2002). Bazeley, G.P., Cheung, W.K., Irons, B.M. and Zienkiewicz, O.C., “Triangular Elements in Plate Bending—Conforming and Nonconforming Solutions in Matrix Methods and Structural Mechanics,” Proc. Conf. on Matrix Methods in Structural Analysis, Rept. AFFDL-R-66-80, Wright Patterson AFB, 547-576 (1965). Belytschko, T., “Transient Analysis,” Structural Mechanics Computer Programs, edited by W. Pilkey, et. al., University Press of Virginia, 255-276 (1974). Belytschko, T., and Bindeman, L. P., "Assumed Strain Stabilization of the Eight Node Hexahedral Element," Comp. Meth. Appl. Mech. Eng. 105, 225-260 (1993). Belytschko, T., and Hsieh, B.J., ”Nonlinear Transient Finite Element Analysis with Convected Coordinates,” Int. J. Num. Meths. Engrg., 7, 255–271 (1973). Belytschko, T., and Leviathan, I., “Projection schemes for one-point quadrature shell elements,” Comp. Meth. Appl. Mech. Eng., 115, 277-286 (1994). Belytschko, T., and Lin, J., “A New Interaction Algorithm with Erosion for EPIC-3”, Contract Report BRL-CR-540, U.S. Army Ballistic Research Laboratory, Aberdeen Proving Ground, Maryland (1985). Belytschko, T., Lin, J., and Tsay, C.S., “Explicit Algorithms for Nonlinear Dynamics of Shells,” Comp. Meth. Appl. Mech. Eng. 42, 225-251 (1984) [a]. Belytschko, T., Ong, J. S.-J., Liu, W.K. and Kennedy, J.M., “Hourglass Control in Linear and Nonlinear Problems”, Comput. Meths. Appl. Mech. Engrg., 43, 251–276 (1984b). Belytschko, T., Stolarski, H., and Carpenter, N., “A C0 Triangular Plate Element with One-Point Quadrature,” International Journal for Numerical Methods in Engineering, 20, 787-802 (1984) [b]. References LS-DYNA Theory Manual Belytschko, T., Schwer, L., and Klein, M. J., “Large Displacement Transient Analysis of Space Frames,” International Journal for Numerical and Analytical Methods in Engineering, 11, 65-84 (1977). Belytschko, T., and Tsay, C.S., “Explicit Algorithms for Nonlinear Dynamics of Shells,” AMD, 48, ASME, 209-231 (1981). Belytschko, T., and Tsay, C.S., “WHAMSE: A Program for Three-Dimensional Nonlinear Structural Dynamics,” Report EPRI NP-2250, Project 1065-3, Electric Power Research Institute, Palo Alto, CA (1982). Belytschko, T., and Tsay, C. S., “A Stabilization Procedure for the Quadrilateral Plate Element with One-Point Quadrature,” Int. J. Num. Method. Eng. 19, 405-419 (1983). Belytschko, T., Yen, H. R., and Mullen R., “Mixed Methods for Time Integration,” Computer Methods in Applied Mechanics and Engineering, 17, 259-175 (1979). Belytschko, T., “Partitioned and Adaptive Algorithms for Explicit Time Integration,” in Nonlinear Finite Element Analysis in Structural Mechanics, ed. by Wunderlich, W. Stein, E, and Bathe, J. J., 572-584 (1980). Belytschko, T., Wong, B.L., and Chiang, H.Y., “Improvements in Low-Order Shell Elements for Explicit Transient Analysis,” Analytical and Computational Models of Shells, A.K. Noor, T. Belytschko, and J. Simo, editors, ASME, CED, 3, 383-398 (1989). Belytschko, T., Wong, B.L., and Chiang, H.Y., “Advances in One-Point Quadrature Shell Elements,” Comp. Meths. Appl. Mech. Eng., 96, 93-107 (1992). Belytschko, T., Wong, B. L., Plaskacz, E. J., "Fission - Fusion Adaptivity in Finite Elements for Nonlinear Dynamics of Shells," Computers and Structures, Vol. 33, 1307- 1323 (1989). Belytschko, T., Lu, Y.Y. and Gu, L., “Element-free Galerkin Methods,” Int. J. Numer. Methods Engrg. 37, 229-256 (1994). Benson, D.J., “Vectorizing the Right-Hand Side Assembly in an Explicit Finite Element Program,” Comp. Meths. Appl. Mech. Eng., 73, 147-152 (1989). Benson, D. J., and Hallquist, J.O., “A Simple Rigid Body Algorithm for Structural Dynamics Program,” Int. J. Numer. Meth. Eng., 22 (1986). Benson, D.J., and Hallquist J.O., “A Single Surface Contact Algorithm for the Postbuckling Analysis of Shell Structures,” Comp. Meths. Appl. Mech. Eng., 78, 141- 163 (1990). LS-DYNA Theory Manual References Benson, D. J., “Momentum Advection on a Staggered Mesh,” Journal of Computational Physics, 100, No. 1, (1992). Benson, D. J., “Vectorization Techniques for Explicit Arbitrary Lagrangian Eulerian Calculations,” Computer Methods in Applied Mechanics and Engineering (1992). Berstad, T., "Material Modelling of Aluminium for Crashworthiness Analysis", Dr.Ing. Dissertation, Department of Structural Engineering, Norwegian University of Science and Technology, Trondheim, Norway (1996). Berstad T., Hopperstad, O.S., and Langseth, M., “Elasto-Viscoplastic Consitiutive Models in the Explicit Finite Element Code LS-DYNA,” Proceedings of the Second International LS-DYNA Conference, San Francisco, CA (1994). Bischoff M. and Ramm E., “Shear deformable shell elements for large strains and rotations,” . Int. J. Numer. Methods, 40, 4427-4449 (1997). Blatz, P.J., and Ko, W.L., “Application of Finite Element Theory to the Deformation of Rubbery Materials,” Trans. Soc. of Rheology, 6, 223-251 (1962). Bodig, Jozsef and Benjamin A. Jayne, Mechanics of Wood and Wood Composites, Krieger Publishing Company, Malabar, FL (1993). Boeing, Boeing Extreme Mathematical Library BCSLIB-EXT User's Guide, The Boeing Company, Document Number 20462-0520-R4 (2000). Borrvall, T., Development and implementation of material tangent stiffnesses for material model 76 in LS-DYNA, ERAB-02:46, Engineering Research Nordic AB, Linköping (2002). Borrvall, T., Revision of the implementation of material 36 for shell elements in LS- DYNA, ERAB Report E0307, Engineering Research Nordic AB, Linköping (2003). Björklund O., “Ductile Failure in High Strength Steel Sheets,” Linköping Studies in Science and Technology. Dissertations No. 1579, ISSN 0345-7524 (2014). Brekelmans, W.A.M., Scheurs, P.J.G., and de Vree, J.H.P., “Continuum damage mechanics for softening of brittle materials”, Acta Mechanica, 93, 133-143, (1991). Brooks, A. N., and Hughes, T. J. R., “Streamline Upwind/Petrov-Galerkin Formulations for Convection Dominated Flows with Particular Emphasis on the Incompressible Navier-Stokes Equations,” Computer Methods in Applied Mechanics and Engineering, 32, 199-259, (1982). References LS-DYNA Theory Manual Burton, D.E., et. al., “Physics and Numerics of the TENSOR Code,” Lawrence Livermore National Laboratory, Internal Document UCID-19428 (July 1982). Cardoso, R.P.R. and Yoon J-W., “One point quadrature shell element with through- thickness stretch, Computer Methods in Applied Mechanics and Engineering,” 194(9), 1161-1199 (2005). Chang, F.K., and Chang, K.Y., “Post-Failure Analysis of Bolted Composite Joints in Tension or Shear-Out Mode Failure,” J. of Composite Materials, 21, 809-833 (1987).[a] Chang, F.K., and Chang, K.Y., “A Progressive Damage Model for Laminated Composites Containing Stress Concentration,” J. of Composite Materials, 21, 834-855 (1987).[b] Chang, F.S., “Constitutive Equation Development of Foam Materials,” Ph.D. Dissertation, submitted to the Graduate School, Wayne State University, Detroit, Michigan (1995). Chang, F.S., J.O. Hallquist, D. X. Lu, B. K. Shahidi, C. M. Kudelko, and J.P. Tekelly, “Finite Element Analysis of Low Density High-Hystersis Foam Materials and the Application in the Automotive Industry,” SAE Technical Paper 940908, in Saftey Technology (SP-1041), International Congress and Exposition, Detroit, Michigan (1994). Chen, J.S., Pan, C., Wu, C.T. and Liu, W.K., “Reproducing Kernel Particle Methods for Large Deformation Analysis of Nonlinear Structures,” Comput. Methods Appl. Mech. Engrg. 139, 195-227 (1996). Chen, J.S. and Wu, C.T., “Generalized Nonlocal Meshfree Method in Strain Localization,” Proceeding of International Conference on Computational Engineering Science, Atlanta, Georiga, 6-9 October (1998). Chen, J.S. and Wang, H.P. “New Boundary Condition Treatmens in Meshfree Computation of Contact Problems,” Computer Methods in Applied Mechanics and Engineering, 187, 441-468, (2001a). Chen, J.S., Wu, C.T., Yoon, S. and You, Y. “A Stabilized Conforming Nodal Integration for Galerkin Meshfree Methods,” Int. J. Numer. Methods Engrg. 50, 435-466 (2001b). Chen, W.F., and Baladi, G.Y., Soil Plasticity: Theory and Implementation, Elesvier, New York, (1985). LS-DYNA Theory Manual References Christensen, R.M. “A Nonlinear Theory of Viscoelasticity for Application to Elastomers,” Journal of Applied Mechanics, 47, American Society of Mechanical Engineers, 762-768 (December 1980). Chung, K., and K. Shah, “Finite Element Simulation of Sheet Metal Forming for Planar Anisotropic Metals,” Int. J. of Plasticity, 8, 453-476 (1992). Cochran, S.G., and Chan, J., “Shock Initiation and Detonation Models in One and Two Dimensions,” University of California, Lawrence Livermore National Laboratory, Rept. UCID-18024 (1979). Cohen, M., and Jennings, P.C., “Silent Boundary Methods for Transient Analysis”, in Computational Methods for Transient Analysis, T. Belytschko and T.J.R. Hughes, editors, North-Holland, New York, 301-360 (1983). Cook, R. D., Concepts and Applications of Finite Element Analysis, John Wiley and Sons, Inc. (1974). Couch, R., Albright, E. and Alexander, “The JOY Computer Code,” University of California, Lawrence Livermore National Laboratory, Rept. UCID-19688 (1983). Cray Research Inc., “CF77 Compiling System, Volume 4: Parallel Processing Guide,” SG-3074 4.0, Mendota Heights, MN (1990). Crisfield M.A., Non-linear Finite Element Analysis of Solids and Structures, Volume 2, Advanced Topics, John Wiley, New York (1997). DeBar, R. B., “Fundamentals of the KRAKEN Code,” Lawrence Livermore Laboratory, UCIR-760 (1974). Deshpande, V.S. and N.A. Fleck, “Isotropic Models for Metallic Foams,” Journal of the Mechanics and Physics of Solids, Vol. 48, 1253-1283, (2000). Dobratz, B.M., “LLNL Explosives Handbook, Properties of Chemical Explosives and Explosive Simulants,” University of California, Lawrence Livermore National Laboratory, Rept. UCRL-52997 (1981). Duff, I. S., and Reid, J. K., "The Multifrontal Solution of Indefinite Sparse Symmetric Linear Equations," ACM Transactions of Mathematical Software, 9, 302-325 (1983). Dvorkin, E.N. and Bathe, K.J. “A continuum mechanics based four-node shell element for general nonlinear analysis,” International Journal for Computer-Aided Engineering and Software, 1, 77-88 (1984). References LS-DYNA Theory Manual Englemann, B.E. and Whirley, R.G., “A New Explicit Shell Element Formulation for Impact Analysis,” In Computational Aspects of Contact Impact and Penetration, Kulak, R.F., and Schwer, L.E., Editors, Elmepress International, Lausanne, Switzerland, 51-90 (1991). Englemann, B.E., Whirley, R.G., and Goudreau, G.L., “A Simple Shell Element Formulation for Large-Scale Elastoplastic Analysis,” In Analytical and Computational Models of Shells, Noor, A.K., Belytschko, T., and Simo, J.C., Eds., CED-Vol. 3, ASME, New York, New York (1989). Farhoomand, I., and Wilson, E.L., “A Nonlinear Finite Element Code for Analyzing the Blast Response of Underground Structures,” U.S. Army Waterways Experiment Station, Contract Rept. N-70-1 (1970). Feng, W.W., Private communication, Livermore, CA (1993). Flanagan, D.P. and Belytschko, T., “A Uniform Strain Hexahedron and Quadrilateral and Orthogonal Hourglass Control,” Int. J. Numer. Meths. Eng. 17, 679-706 (1981) Fleck, J.T., “Validation of the Crash Victim Simulator,” I - IV, Report No. DOT-HS-806 279 (1981). Fleischer M., Borrvall T., and Bletzinger K-U., “Experience from using recently implemented enhancements for Material 36 in LS-DYNA 971 performing a virtual tensile test”, 6th European LS-DYNA Users Conference, Gothenburg, Sweden, 2007. “Fundamental Study of Crack Initiation and Propagation,” Author unknown, LLNL report, document received from LSTC (2003). Galbraith, P.C., M.J. Finn, S.R. MacEwen, et.al., "Evaluation of an LS-DYNA3D Model for Deep-Drawing of Aluminum Sheet", FE-Simulation of 3-D Sheet Metal Forming Processes in Automotive Industry, VDI Berichte, 894, 441-466 (1991). Ghanem RG, Spanos PD. Stochastic Finite Elements – A Spectral Approach, Springer- Verlag, 1991, Revised Edition, Dover, 2003. Ginsberg, M. and Johnson, J.P., “Benchmarking the Performance of Physical Impact Simulation Software on Vector and Parallel Computers,” Proc. of the Supercomputing 88: Vol. II, Science and Applications, Computer Society Press (1988). Gingold, R.A., and Monaghan, J.J., “Smoothed Particle Hydrodynamics: Theory and Application to Non-Spherical Stars,” Mon. Not. R. Astron. Soc. 181, 375-389 (1977). LS-DYNA Theory Manual References Ginsberg, M., and Katnik, R.B., “Improving Vectorization of a Crashworthiness Code,” SAE Technical Paper No. 891985, Passenger Car Meeting and Exposition, Dearborn, MI (1989). Giroux, E.D., “HEMP User's Manual,” University of California, Lawrence Livermore National Laboratory, Rept. UCRL-51079 (1973). Govindjee, S., Kay G.J., and Simo, J.C., “Anisotropic Modeling and Numerical Simulation of Brittle Damage in Concrete,” Report Number UCB/SEM M-94/18, University of California at Berkeley, Department of Civil Engineering (1994). Govindjee, S., Kay G.J., and Simo, J.C., “Anisotropic Modeling and Numerical Simulation of Brittle Damage in Concrete,” International Journal for Numerical Methods in Engineering, Volume 38, pages 3611-3633 (1995). Green, A.E. and Naghdi, P.M., “A General Theory of Elastic-Plastic Continuum,” Archive for Rational Mechanics and Analysis, 18, 251 (1965). Groenwold, A.A. and Stander, N. An efficient 4-node 24 d.o.f. thick shell finite element with 5-point quadrature. Eng. Comput. 12(8), 723-747, 1995. Grimes, Roger, Lewis, John G., and Simon, Horst D., "A Shifted Block Lanczos Algorithm for Solving Sparse Symmetric Generalized Eigenproblems," SIAM Journal of Matrix Analyis and Applications, 15, 228-272 (1994). Guccione, J., A. McCulloch, and L. Waldman, "Passive Material Properties of Intact Ventricular Myocardium Determined from a Cylindrical Model," published in the ASME Journal of Biomechanical Engineering, 113, 42-55 (1991). Hallquist, J.O., “Preliminary User’s Manuals for DYNA3D and DYNAP (Nonlinear Dynamic Analysis of Solids in Three Dimension),” University of California, Lawrence Livermore National Laboratory, Rept. UCID-17268 (1976) and Rev. 1 (1979).[a] Hallquist, J.O., “A Procedure for the Solution of Finite Deformation Contact-Impact Problems by the Finite Element Method,” University of California, Lawrence Livermore National Laboratory, Rept. UCRL-52066 (1976). Hallquist, J.O., “A Numerical Procedure for Three-Dimensional Impact Problems,” American Society of Civil Engineering, Preprint 2956 (1977). Hallquist, J.O., “A Numerical Treatment of Sliding Interfaces and Impact,” in: K.C. Park and D.K. Gartling (eds.) Computational Techniques for Interface Problems, AMD, 30, ASME, New York (1978). References LS-DYNA Theory Manual Hallquist, J.O., “NIKE2D: An Implicit, Finite-Element Code for Analyzing the Static and Dynamic Response of Two-Dimensional Solids,” University of California, Lawrence Livermore National Laboratory, Rept. UCRL-52678 (1979).[b] Hallquist, J.O. (1998), LS-DYNA Theoretical Manual, May (1998). Hallquist, J.O., “User's Manual for DYNA2D— An Explicit Two-Dimensional Hydrodynamic Finite Element Code with Interactive Rezoning,” University of California, Lawrence Livermore National Laboratory, Rept. UCID-18756 (1980). Hallquist, J.O., “User's Manual for DYNA3D and DYNAP (Nonlinear Dynamic Analysis of Solids in Three Dimensions),” University of California, Lawrence Livermore National Laboratory, Rept. UCID-19156 (1981).[a] Hallquist, J. O., “NIKE3D: An Implicit, Finite-Deformation, Finite-Element Code for Analyzing the Static and Dynamic Response of Three-Dimensional Solids,” University of California, Lawrence Livermore National Laboratory, Rept. UCID-18822 (1981).[b] Hallquist, J.O., “DYNA3D User's Manual (Nonlinear Dynamic Analysis of Solids in Three Dimensions),” University of California, Lawrence Livermore National Laboratory, Rept. UCID-19156 (1982; Rev. 1: 1984; Rev. 2: 1986). Hallquist, J.O., “Theoretical Manual for DYNA3D,” University of California, Lawrence Livermore National Laboratory, Rept. UCID-19401 (March, 1983). Hallquist, J.O., “DYNA3D User's Manual (Nonlinear Dynamic Analysis of Solids in Three Dimensions),” University of California, Lawrence Livermore National Laboratory, Rept. UCID-19156 (1988, Rev. 4). Hallquist, J.O., “DYNA3D User's Manual (Nonlinear Dynamic Analysis of Solids in Three Dimensions),” Livermore Software Technology Corporation, Rept. 1007 (1990). Hallquist, J.O., LS-DYNA Keyword User’s Manual, version 970, Livermore Software Technology Corporation (April, 2003). Hallquist, J.O., Benson, D.J., and Goudreau, G.L., “Implementation of a Modified Hughes-Liu Shell into a Fully Vectorized Explicit Finite Element Code,” Proceedings of the International Symposium on Finite Element Methods for Nonlinear Problems, University of Trondheim, Trondheim, Norway (1985). Hallquist, J.O., and Benson, D.J., “A Comparison of an Implicit and Explicit Implementation of the Hughes-Liu Shell,” Finite Element Methods for Plate and Shell LS-DYNA Theory Manual References Structures, T.J.R. Hughes and E. Hinton, Editors, 394-431, Pineridge Press Int., Swanea, U.K. (1986). Hallquist, J.O., and Benson, D.J., “DYNA3D User’s Manual (Nonlinear Dynamic Analysis of Solids in Three Dimensions),” University of California, Lawrence Livermore National Laboratory, Rept. UCID-19156 (1986, Rev. 2). Hallquist, J.O. and Benson, D.J., “DYNA3D User’s Manual (Nonlinear Dynamic Analysis of Solids in Three Dimensions),” University of California, Lawrence Livermore National Laboratory, Rept. UCID-19156 (1987, Rev. 3). Hallquist, J.O., Stillman, D.W., Hughes, T.J.R., and Tarver, C.,”Modeling of Airbags Using MVMA/DYNA3D,” LSTC Report (1990). Harten, A., “ENO Schemes with Subcell Resolution,” J. of Computational Physics, 83, 148-184, (1989). Hashin, Z, “Failure Criteria for Unidirectional Fiber Composites,” Journal of Applied Mechanics, 47, 329 (1980). Herrmann, L.R. and Peterson, F.E., “A Numerical Procedure for Viscoelastic Stress Analysis,” Seventh Meeting of ICRPG Mechanical Behavior Working Group, Orlando, FL, CPIA Publication No. 177 (1968). Hill A.V., "The heat of shortening and the dynamic constants of muscle," Proc Roy Soc B126:136-195, (1938). Hill, R., “A Theory of the Yielding and Plastic Flow of Anisotropic Metals,” Proceedings of the Royal Society of London, Series A., 193, 281 (1948). Hill, R. “Consitiutive Modeling of Orthotropic Plasticity in Sheet Metals,” Journal of Mechanics and Physics of Solids, 38, Number 3, 405-417 (1999). Holmquist, T.J., G.R. Johnson, and W.H. Cook, "A Computational Constitutive Model for Concrete Subjected to Large Strains, High Strain Rates, and High Pressures, pp. 591- 600, (1993). Holtz R.D., W. D. Kovacs, “ An Introduction to Geotechnical Engineering”, Prentice Hall, Inc. New Jersey, 1981 Hopperstad, O.S. and Remseth, S., “A Return Mapping Algorithm for a Class of Cyclic Plasticity Models,” International Journal for Numerical Methods in Engineering, 38, 549-564 (1995). References LS-DYNA Theory Manual Hughes, T.J.R., The Finite Element Method, Linear Static and Dynamic Finite Element Analysis, Prentice-Hall Inc., Englewood Cliffs, NJ (1987). Hughes, T.J.R., “Generalization of Selective Integration Procedures to Anisotropic and Nonlinear Media,” Int. J. Numer. Meth. Eng. 15, 9 (1980). Hughes, T.J.R. and Carnoy, E., “Nonlinear Finite Element Shell Formulation Accounting for Large Membrane Strains,” AMD-Vol.48, ASME, 193-208 (1981). Hughes, T.J.R. and Liu, W.K., “Nonlinear Finite Element Analysis of Shells: Part I. Two-Dimensional Shells.” Comp. Meths. Appl. Mechs. 27, 167-181 (1981). Hughes, T.J.R. and Liu, W.K., “Nonlinear Finite Element Analysis of Shells: Part II. Three-Dimensional Shells.” Comp. Meths. Appl. Mechs. 27, 331-362 (1981). Hughes, T.J.R., Liu,W.K., and Levit, I., “Nonlinear Dynamics Finite Element Analysis of Shells.” Nonlinear Finite Element Analysis in Struct. Mech., Eds. W. Wunderlich, E. Stein, and K.J. Bathe, Springer-Verlag, Berlin, 151–168 (1981). Hughes, T.J.R., Taylor, R. L., Sackman, J. L., Curnier, A.C., and Kanoknukulchai, W., “A Finite Element Method for a Class of Contact-Impact Problems,” J. Comp. Meths. Appl. Mechs. Eng. 8, 249-276 (1976). Hughes, T.J.R., and Winget, J., “Finite Rotation Effects in Numerical Integration of Rate Constitutive Equations Arising in Large-Deformation Analysis,” Int. J. Numer. Meths. Eng., 15, 1862-1867, (1980). Hulbert, G.M. and Hughes, T.J.R., “Numerical Evaluation and Comparison of Subcycling Algorithms for Structural Dynamics,” Technical Report, DNA-TR-88-8, Defense Nuclear Agency, Washington, DC (1988). Ibrahimbegovic, A. and Wilson, E.L. A unified formulation for triangular and quadrilateral flat shell finite elements with six nodal degrees of freedom, Comm. Applied Num. Meth, 7, 1-9, 1991. Isenberg, J., D.K. Vaughn, and I. Sandler, "Nonlinear Soil-Structure Interaction," EPRI Report MP-945, Weidlinger Associates, December (1978). Jabareen, M., and Rubin, M.B., A Generalized Cosserat Point Element (CPE) for Isotropic Nonlinear Elastic Materials including Irregular 3-D Brick and Thin Structures, J. Mech. Mat. And Struct., Vol 3-8, 1465-1498 (2008). LS-DYNA Theory Manual References Jabareen, M., Hanukah, E. and Rubin, M.B., A Ten Node Tetrahedral Cosserat Point Element (CPE) for Nonlinear Isotropic Elastic Materials, J. Comput. Mech. 52, 257-285 (2013). Jaumann, G. “Geschlossenes System Physikalischer und Chemischer Differentialdesefz, Sitz Zer. Akad. Wiss. Wein, (IIa), 120, 385 (1911). Johnson, G.C. and Bammann D.J., “A Discussion of Stress Rates in Finite Deformation Problems" International Journal of Solids and Structures, 20, 725-737 (1984). Johnson, G.R. and Cook,W. H., “A Constitutive Model and Data for Metals Subjected to Large Strains, High Strain Rates and High Temperatures,” presented at the Seventh International Symposium on Ballistics, The Hague, The Netherlands, April (1983). Johnson, G.R. and T.J. Holmquist, "An Improved Computational Model for Brittle Materials" in High-Pressure Science and Technology - 1993 American Institute of Physics Conference Proceedings 309 (c 1994) pp.981-984 ISBN 1-56396-219-5. Johnson, C., Navert, U., and Pitkaranta, J., “Finite Element Methods for Linear Hyperbolic Problems,” Computer Methods in Applied Mechanics and Engineering, 45, 285-312, (1984). Jones, N., “Structural Aspects of Ship Collisions,” Chapter 11, in Structural Crashworthiness, Eds. N. Jones and T Wierzbicki, Butterworths, London, 308-337 (1983). Jones, R.M., Mechanics of Composite Materials, Hemisphere Publishing Co., New York (1975). Ju J.W., “Energy-Based Coupled Elastoplastic Damage Models at Finite Strains”, J. of Eng Mech., Vol 115, No 11, Nov 1989. Karypis, G., and Kumar V., "METIS: A Software Package for Partitioning Unstructured Graphs, Partitioning Meshes, and Computing Fill-Reducing Orderings of Sparse Matrices," Department of Computer Science, University of Minnesota (1998). Katz, J., and Maskew, B., “Unsteady Low-Speed Aerodynamic Model for Complete Aircraft Configurations,” Journal of Aircraft 25, 4 (1988). Kenchington, G. J., “A Non-Linear Elastic Material Model for DYNA3D,” Proceedings of the DYNA3D Users Group Conference, September 1988, published by Boeing Computer Services (Europe) Limited. References LS-DYNA Theory Manual Kennedy, J. M., Belytschko,T., and Lin, J. I., “Recent Developments in Explicit Finite Element Techniques and their Applications to Reactor Structures,” Nuclear Engineering and Design 97, 1-24 (1986). Kim, N., Seo, K., and Kim, M., “Free Vibration and Spatial Stability of Non-symmetric Thin-Walled Curved Beams with Variable Curvatures,” International Journal of Solids and Structures, 40, 3107-3128, (2003). Klisinski M., “Degradation and Plastic Deformation of Concrete”, Ph.D. thesis, Polish Academy of Sciences, 1985, IFTR report 38. Kosloff, D. and Frazier, G.A.,“Treatment of Hourglass Patterns in Low Order Finite Element Codes,” Int. J. Numer. Anal. Meth. Geomech. 2, 57-72 (1978) Kretschmann, D. E., and David W. Green, “Modeling Moisture Content-Mechanical Property Relationships for Clear Southern Pine,” Wood and Fiber Science, 28(3), pp. 320-337 (1996). Kreyszig, E., Advanced Engineering Mathematics, John Wiley and Sons, New York, New York (1972). Krieg, R.D.,”A Simple Constitutive Description for Cellular Concrete,” Sandia National Laboratories, Albuquerque, NM, Rept. SC-DR-72-0883 (1972). Krieg, R.D. and Key, S.W., Implementation of a Time Dependent Plasticity Theory into Structural Computer Programs, Vol. 20 of Constitutive Equations in Viscoplasticity: Computational and Engineering Aspects (American Society of Mechanical Engineers, New York, N.Y., 1976), 125-137. Kumar, P., Nukala, V. V., and White, D. W., “A Mixed Finite Element for Three- dimensional Nonlinear Analysis of Steel Frames,” Computational Methods in Applied Mechanical Engineering, 193, 2507-2545, (2004). Lancaster, P. and Salkauskas, K., “Surfaces generated by moving least squares methods”, Math. Comput. 37, 141-158, (1981). Landshoff, R., “A Numerical Method for Treating Fluid Flow in the Presence of Shocks,” Los Alamos Scientific Laboratory, Rept. LA-1930 (1955). Lee, E.L. and Tarver, C.M., “Phenomenological Model of Shock Initiation in Heterogeneous Explosives,” Phys. of Fluids, 23, 2362 (1980). LS-DYNA Theory Manual References Lemaitre, J., A Course on Damage Mechanics. Springer-Verlag, (1992). Lemmen, P.P.M and Meijer, G.J., “Failure Prediction Tool Theory and User Manual,” TNO Building and Construction Research, The Netherlands, Rept. 2000-CMC-R0018, (2001). Lewis B.A., “Developing and Implementing a Road Side Safety Soil Model into LS- DYNA”, FHWA Research and Development Turner-Fairbank Highway Research Center. Oct, 1999. Librescu, L. Qin, Z., and Ambur D.R., “Implications of Warping Restraint on Statics and Dynamics of Elastically Tailored Thin-Walled Composite Beams,” International Journal of Mechanical Sciences, 45, 1247-1267 (2003). Liu, Joseph W. H., "Modification of the Minimum-Degree Algorithm by Multiple Elimination," ACM Transactions on Mathematical Software, 11, 141-153 (1985). Liu, W.K. and Belytschko, T., “Efficient Linear and Nonlinear Heat Conduction with a Quadrilateral Element,” Int. J. Num. Meths. Engrg., 20, 931–948 (1984). Liu, W.K., Belytschko, T., Ong, J.S.J. and Law, E., “Use of Stabilization Matrices in Nonlinear Finite Element Analysis,” Engineering Computations, 2, 47–55 (1985). Liu, W.K., Lecture Notes on Nonlinear Finite Element Methods, Northwestern University, (1983, revised in 1992). Liu, W.K., Guo, Y., Tang, S. and Belytschko T., “A Multiple-Quadrature Eight-node Hexahedral Finite Element for Large Deformation Elastoplastic Analysis,” Comput. Meths. Appl. Mech. Engrg., 154, 69–132 (1998). Liu, W.K., Hu, Y.K., and Belytschko, T., “Multiple Quadrature Underintegrated Finite Elements,” Int. J. Num. Meths. Engrg., 37, 3263–3289 (1994). Liu, W. K., Chang, H., and Belytschko, T., “Arbitrary Lagrangian-Eulerian Petrov- Galerkin Finite Elements for Nonlinear Continua,” Computer Methods in Applied Mechanics and Engineering, to be published. Liu, W.K., Jun, S. and Zhang, Y.F., “Reproducing Kernel Particle Method,” Int. J. Numer. Methods Fluids 20, 1081-1106 (1995). Lucy, L.B., “Numerical Approach to Testing the Fission Hyphothesis,” Astron. J. 82, 1013-1024 (1977). References LS-DYNA Theory Manual Lysmer, J. and Kuhlemeyer, R.L., “Finite Dynamic Model for Infinite Media”, J. Eng. Mech. Div. ASCE, 859-877 (1969). MacNeal R.H. and Harder R.L., “A Proposed Standard Set of Problems to Test Finite Element Accuracy,” Finite Elements Anal. Des., (1985, 3–20 (1985). Maenchen, G. and Sack, S., “The Tensor Code,” Meth. Comp. Phys. 3, (Academic Press), 181-263 (1964). Maffeo, R., “TRANCITS Program User’s Manual,” General Electric Company, Cincinnati, OH, NASA Report CR-174891, (1985). Maffeo, R., “Burner Liner Thermal/Structural Load Modeling,” General Electric Company, Cincinnati, OH, NASA Report CR-174892, (1984). Maker, B. N., Private communication, Lawrence Livermore National Laboratory. Dr. Maker programmed and implemented the compressible Mooney-Rivlin rubber model. Marchertas, A. H., and Belytschko,T. B., “Nonlinear Finite Element Formulation for Transient Analysis of Three Dimensional Thin Structures,” Report ANL-8104, LMFBR Safety, Argonne National Laboratory, Argonne, IL (1974). Margolin, L. G., personal communication to D. Benson (1989). Maskew, B., “Program VSAERO Theory Document,” NASA CR-4023 (1987). Matthies, H., and G. Strang, The Solution of Nonlinear Finite Element Equations, Int., Journal for Numerical Methods in Engineering, 14, No. 11, 1613-1626. Matzenmiller, A., and Schweizerhof, K., “Crashworthiness Simulatios of Composite Structures - A First Step with Explicit Time Integration,” Nonlinear Computational mechanics - A State of the Art, edited by P.W. Wriggers, et. al., Springer-Verlag, (1991). Mauldin, P.J., R.F. Davidson, and R.J. Henninger, “Implementation and Assessment of the Mechanical-Threshold-Stress Model Using the EPIC2 and PINON Computer Codes,” Report LA-11895-MS, Los Alamos National Laboratory (1990). McGlaun, personal communication to D. Benson, Sandia National Laboratories, (1990). McGlaun, J. M., Thompson, S. L., and Elrick, M. G., ”CTH: A Three-Dimensional Shock Wave Physics Code,” Proc. of the 1989 Hypervelocity Impact Symposium (1989). Mindlin, R.D., “Influence of Rotary Inertia and Shear on Flexural Motions of Isotropic, Elastic Plates,” J. Appl. Mech. 18, 31-38 (1951). LS-DYNA Theory Manual References Mizukami, A., and Hughes, T. J. R., “A Petrov-Galerkin Finite Element Method for Convection Dominated Flows: An Accurate Upwinding Technique for Satisfying the Maximum Principle,” Computer Methods in Applied Mechanics and Engineering, Vol. 50, pp. 181-193 (1985). Monaghan, J.J., and Gingold, R.A., “Shock Simulation by the Particle Method of SPH,” Journal of Computational Physics, 52, 374-381 (1983). Murray Y.D., “Modeling Rate Effects in Rock and Concrete”, Proceedings of the 8th International Symposium on Interaction of the Effects of Munitions with Structures, Defense Special Weapons Agency, McLean VA, USA, (1997). Murray, Y. D., “Modeling Rate Effects in Rock and Concrete,” Proceedings of the 8th International Symposium on Interaction of the Effects of Munitions with Structures, Defense Special Weapons Agency, McLean, VA, USA, (1997). Murray, Y.D., Users Manual for Transversely Isotropic Wood Model, aptek technical report to fhwa (to be published), (2002). Murray, Y.D., and J. Reid, Evaluation of Wood Model for Roadside Safety Applications, aptek technical report to fhwa (to be puslished), (2002). Nagtegaal, J.C., Parks, D.M., and Rice J.R., “On Numerically Accurate Finite Element Solution in the Fully Plastic Range”, Computer Methods in Applied Mechanics and Engineering, 4, 153 (1974). Newman, W.M., and Sproull, R.F., Principles of Interactive Computer Graphics, McGraw-Hill, New York (1979). Newmark, N., “A Method of Computation for Structural Dynamics,” Journal of the Engineering Mechanics Division, Proceedings of the American Society of Civil Engineers, 67-94 (1959). Neilsen, M.K., Morgan, H.S., and Krieg, R.D., “A Phenomenological Constitutive Model for Low Density Polyurethane Foams,” Rept. SAND86-2927, Sandia National Laboratories, Albuquerque, NM (1987). Noh, W.F., Meth. Comp. Phys. 3, (Academic Press) (1964). Noh, W.F., “Numerical Methods in Hydrodynamic Calculations,” University of California, Lawrence Livermore National Laboratory, Rept. UCRL-52112 (1976). Oden, J.T, P. Devloo, and T. Strouboulis, "Adaptive Finite Element Methods for the Analysis of Inviscid Compressible Flow: Part I. Fast Refinement/Unrefinement and References LS-DYNA Theory Manual Moving Mesh Methods for Unstructured Meshes," Computer Methods in Applied Mechanics and Engineering, 59, 327-362 (1986). Ogden, R.W., Non-Linear Elastic Deformations, Ellis Horwood Ltd., Chichester, Great Britian (1984). Okuda T., Yamamae Y. and Yasuki T., Request for MAT126 Modification, Microsoft Power Point presentation, Toyota Communication Systems and Toyota Motor Corporation, 2003. Oliver, J., “A Consistent Characteristic Length of Smeared Cracking Models,” International Journal for Numerical Methods in Engineering, 28, 461-474 (1989). Rajendran, A.M.,"Material Failure Models", in Material Behavior at High Strain Rates, Course Notes, Computational Mechanics Associates, Monterey, CA, 424 (1989). Papadrakakis, M., “A Method for the Automated Evaluation of the Dynamic Relaxation Parameters,” Comp. Meth. Appl. Mech. Eng. 25, 35-48 (1981). Phoon KK, Huang SP, Quek ST. Implementation of Karhunen–Loeve expansion for simulation using a wavelet-Galerkin scheme. Probabilist Eng Mech 2002;17(3):293–303. (2002a) Phoon KK, Huang SP, Quek ST. Simulation of second-order processes using Karhunen– Loeve expansion. Comput Struct 2002; 80(12):1049–60. (2002b) Phoon KK, Huang HW, Quek ST. Simulation of strongly non-Gaussian processes using Karhunen–Loeve expansion, Probabilistic Engineering Mechanics 20 (2005) 188–198. Pian, T.H.H., and Sumihara, K., “Rational Approach for Assumed Stress Elements,” Int. J. Num. Meth. Eng., 20, 1685-1695 (1985). Prokic, A., “New Warping Function for Thin-Walled Beams. I: Theory,” Journal of Structural Engineering, 122, 1437-1442, (1994). Przemieniecki, J. S., Theory of Matrix Structural Analysis, McGraw-Hill Book Company, New York, NY (1986). Reid, S.R. and C. Peng, “Dynamic Uniaxial Crushing of Wood,” Int. J. Impact Engineering, Vol. 19, No. 5-6, pp. 531-570, (1997). Reyes, A., O.S. Hopperstad, T. Berstad, and M. Langseth, “Implementation of a Material Model for Aluminium Foam in LS-DYNA”, Report R-01-02, Restricted, Department of Structural Engineering, Norwegian University of Science and Technology, (2002). LS-DYNA Theory Manual References Richards, G.T., “Derivation of a Generalized von Neumann Pseudo-Viscosity with Directional Properties,” University of California, Lawrence Livermore National Laboratory, Rept. UCRL-14244 (1965). Richtmyer, R.D., and Morton, K.W., Difference Equations for Initial-Value Problems, Interscience Publishers, New York (1967). Sandler, I.S., and D. Rubin, “An Algorithm and a modular subroutine for the cap model,” Int. J. Numer. Analy. Meth. Geomech., 3, 173-186 (1979). Schwer, L.E., Cheva, W., and Hallquist, J.O., “A Simple Viscoelastic Model for Energy Absorbers Used in Vehicle-Barrier Impacts,” In Computational Aspects of Contact Impact and Penetration, Kulak, R.F., and Schwer, L.E., Editors, Elmepress International, Lausanne, Switzerland, 99-117 (1991). Shapiro, A.B., “TOPAZ3D - A Three Dimensional Finite Element Heat Transfer Code,” University of California, Lawrence Livermore National Laboratory, Report UCID-20481 (1985). Shapiro, A.B., “REMAP: a Computer Code That Transfers Node Information Between Dissimilar Grids,” Lawrence Livermore National Laboratory, UCRL-ID-104090, (1990). Shkolnikov, M.B. Private Communication (1990-1991). Simo, J.C. and Govindjee, S., ``Exact Closed-Form Solution of the Return Mapping Algorithm in Plane Stress Elasto-Viscoplasticity," Engineering Computations, 5, 254-258 (1988). Simo, J.C. and Hughes, T.J.R. “On the variational foundations of assumed strain methods,” Journal of Applied Mechanics, 53, 1685-1695 (1986). Simo, J.C., Ju, J.W., “Stress and Strain Based Continuum Damage Models”, Parts I & II, Int. J. of Solids and Structures, Vol 23, No 7, (1987). Simo, J.C., Ju, J.W., Pister, K.S., and Taylor, R.L. “An Assessment of the Cap Model: Consistent Return Algorithms and Rate-Dependent Extension,” J. Eng. Mech., 114, No. 2, 191-218 (1988a). Simo, J.C., Ju, J.W., Pister, K.S., and Taylor, R.L. “Softening Response, Completeness Condition, and Numerical Algorithms for the Cap Model,” Int. J. Numer. Analy. Meth. Eng. (1990). References LS-DYNA Theory Manual Simo, J.C. and Taylor, R.L., “A Return Mapping Algorithm for Plane Stress Elastoplasticity,” International Journal for Numerical Methods in Engineering, 22, 649-670 (1986). Steinberg, D.J. and Guinan, M.W., “A High-Strain-Rate Constitutive Model for Metals,” University of California, Lawrence Livermore National Laboratory, Rept. UCRL-80465 (1978). Stillman, D. W., and Hallquist, J. O., “LS-INGRID: A Pre-Processor and Three- Dimensional Mesh Generator for the Programs LS-DYNA, LS-NIKE3D, and TOPAZ3D,” Version 3.1, Livermore Software Technology Corporation (1992). Stojko, S., privated communication, NNC Limited, Engineering Development Center (1990). Stolarski, H., and Belytschko, T., “Shear and Membrane Locking in Curved Elements,” Comput. Meths. Appl. Mech. Engrg., 41, 279–296 (1983). Stone, C.M., Krieg, R.D., and Beisinger, Z.E., “Sancho, A Finite Element Computer Program for the Quasistatic, Large Deformation, Inelastic Response of Two- Dimensional Solids,” Sandia Report, SAND 84-2618, UC-32, Albuquerque, NM (1985). Storakers, B., “On Material Representation and Constitutive Branching in Finite Compressible Elasticity”, Royal Institute of Technology, Stockholm Sweden, (1985). Sturt, R.M.V., and B.D. Walker, J.C. Miles, A. Giles, and N. Grew, “Modelling the Occupant in a Vehicle Context-An Integrated Approach,” 13th International ESV Conference, Paris, November 4-7 (1991). Sussman, T. and Bathe, K.J., “A Finite Element Formulation for Nonlinear Incompressi- ble Elastic and Inelastic Analysis,” Computers & Structures, 26, Number 1/2, 357-409 (1987). Tarver, C.M., and Hallquist, J.O., “Modeling of Two-Dimensional Shock Initiation and Detonation Wave Phenomena in PBX 9404 and LX-17,” University of California, Lawrence Livermore National Laboratory, Rept. UCID84990 (1981). Taylor, R.L. and Simo, J.C. Bending and membrane elements for the analysis of thick and thin shells, Proc. of NUMETA Conference, Swansea, 1985. Taylor, R.L., Finite element anlysis of linear shell problems, in Whiteman, J.R. (ed.), Proc. of the Mathematics in Finite Elements and Applications, Academic Press, New York, 191-203 (1987). LS-DYNA Theory Manual References Taylor, L.M., and Flanagan, D.P., “PRONTO3D A Three-Dimensional Transient Solid Dynamics Program,” Sandia Report: SAND87-1912, UC-32 (1989). Thompson, S. L., “CSQ -- A Two Dimensional Hydrodynamic Program with Energy Flow and Material Strength,” Sandia Laboratories, SAND74-0122 (1975). Thompson, R., L., and Maffeo, R. L., “A Computer Analysis Program for Interfacing Thermal and Structural Codes,” NASA Lewis Research Center, Report NASA-TM- 87021 (1985). Trefethen, L.N., “Group Velocity in Finite Difference Schemes,” SIAM Review, 24, No. 2 (1982). Tsai, S.W., and Wu, E.M., “A General Theory of Strength for Anisotropic Materials,” Journal of Composite Materials, 58-80 (1971). Tuler, F.R. and B.M. Butcher, "A Criterion for the Time Dependence of Dynamic Fracture," The International Journal of Fracture Mechanics, 4, No. 4 (1968). Turk M, Pentland A. Eigenfaces for Recognition, Journal of Cognitive Neuroscience, 1991; 3(1):71-86. Turkalj, G. Brnic, J., and Prpic-Orsic J., “Large Rotation Analysis of Elastic Thin-Walled Beam-Type Structures Using ESA Approach,” Computers & Structures, 81, 1851-1864, (2003). Underwood, P., “Dynamic Relaxation,” Computational Method for Transient Analysis, Belytschko, T., and Hughes, T.J.R., Eds., 1, 245-263, (1986). Van Leer, B., “Towards the Ultimate Conservative Difference Scheme. IV. A New Approach to Numerical Convection,” Journal of Computational Physics, 23, 276-299 (1977). Vawter, D., "A Finite Element Model for Macroscopic Deformation of the Lung," published in the Journal of Biomechanical Engineering, 102, 1-7, (1980). von Neumann, J., and Richtmyer, R.D., “A Method for the Numerical Calculation of Hydrodynamical Shocks,” J. Appl. Phys., 21, 232 (1950). Walker, B.D., and P.R.B. Dallard, “An integrated Approach to Vehicle Crashworthiness and Occupant Protection Systems”, SAE International Congress and Exposition, Detroit, Michigan, (910148), February 25-March 1 (1991). References LS-DYNA Theory Manual Walker, H.F., Numerical Solution of Nonlinear Equations, University of California, Lawrence Livermore National Laboratory, Rept. UCID-18285 (1979). Wang, J. T., and O. J. Nefske, “A New CAL3D Airbag Inflation Model,” SAE paper 880654, (1988). Wang, J. T., private communication (1992). Wang, J.T., "An Analytical Model for an Airbag with a Hybrid Inflator", Publication R&D 8332, General Motors Development Center, Warren, MI (1995). Wang, J.T., "An Analytical Model for an Airbag with a Hybrid Inflator", AMD-Vol. 210, BED 30, ASME, 467-497 (1995). Warsi, Z. U. A., “Basic Differential Models for Coordinate Generation,” in Symposium on the Numerical Generation of Curvilinear Coordinate Systems, Nashville, Tenn. (1982). Whirley, R. G., Hallquist, J. O., and Goudreau, G. L., “An Assessment of Numerical Algorithms for Plane Stress and Shell Elastoplasticity on Supercomputers,” Engineering Computations, 6, 116-126 (June, 1989). Wilkins, M.L., “Calculations of Elastic Plastic Flow,” Meth. Comp. Phys., 3, (Academic Press), 211-263 (1964). Wilkins, M. L., “Calculation of Elastic-Plastic Flow,” University of California, Lawrence Livermore National Laboratory, Rept. UCRL-7322, Rev. I (1969). Wilkins, M.L., “Use of Artificial Viscosity in Multidimensional Fluid Dynamic Calculations,” J. Comp. Phys. 36, 281 (1980). Wilkins, M.L., Blum, R.E., Cronshagen, E., and Grantham, P., “A Method for Computer Simulation of Problems in Solid Mechanics and Gas Dynamics in Three Dimensions and Time,” University of California, Lawrence Livermore National Laboratory, Rept. UCRL-51574 (1974). Wilson, E.L., Three Dimensional Static and Dynamic Analysis of Structures, A publication of Computers and Structures, Inc., Berkeley, California, [1996-2000]. Winslow, A. M., “Equipotential Zoning of Two-Dimensional Meshes,” Lawrence Radiation Laboratory, UCRL-7312 (1963). Winslow, A. M., “Equipotential Zoning of The Interior of a Three-Dimensional Mesh,” Report to LSTC (1990). LS-DYNA Theory Manual References Winters, J.M., "Hill-based muscle models: A systems engineering perspective," In Multiple Muscle Systems: Biomechanics and Movement Organization, JM Winters and SL-Y Woo eds, Springer-Verlag (1990). Winters J.M. and Stark L., "Estimated mechanical properties of synergistic muscles involved in movements of a variety of human joints,": J Biomechanics 21:1027-1042, (1988). Woodruff, J.P., “KOVEC User’s Manual,” University of California, Lawrence Livermore National Laboratory, Rept. UCRL-51079 (1973). Yen, C.F. and Caiazzo, A, “Innovative Processing of Multifunctional Composite Armor for Ground Vehicles,” ARL-CR-484, U.S. Army Research Laboratory, Aberdeen Proving Ground, MD, (2001). Yunus, S.M., Pawlak, T.P., and Cook, R.D., “ Solid Elements with Rotational Degrees of Freedom, Part I-Hexahedron Elements,” To be published, (1989). Zajac F.E., "Muscle and tendon: Properties, models, scaling, and application to biomechanics and motor control, "CRC Critical Reviews in Biomedical Engineering 17(4):359-411, (1989). References LS-DYNA Theory Manual Corporate Address Livermore Software Technology Corporation P. O. Box 712 Livermore, California 94551-0712 Support Addresses Livermore Software Technology Corporation 7374 Las Positas Road Livermore, California 94551 Tel: 925-449-2500 Fax: 925-449-2507 Email: sales@lstc.com Website: www.lstc.com Disclaimer Technology Software Livermore Corporation 1740 West Big Beaver Road Suite 100 Troy, Michigan 48084 Tel: 248-649-4728 Fax: 248-649-6328 Copyright © 1992-2017 Livermore Software Technology Corporation. All Rights Reserved. LS-DYNA®, LS-OPT® and LS-PrePost® are registered trademarks of Livermore Software Technology Corporation in the United States. All other trademarks, product names and brand names belong to their respective owners. LSTC reserves the right to modify the material contained within this manual without prior notice. The information and examples included herein are for illustrative purposes only and are not intended to be exhaustive or all-inclusive. LSTC assumes no liability or responsibility whatsoever for any direct of indirect damages or inaccuracies of any type or nature that could be deemed to have resulted from the use of this manual. Any reproduction, in whole or in part, of this manual is prohibited without the prior LS-DYNA MULTIPHYSICS USER’S MANUAL INTRODUCTION In this manual, there are three main solvers: a compressible flow solver, an incompressible flow solver, and an electromagnetism solver. Each of them implements coupling with the structural solver in LS-DYNA. The keywords covered in this manual fit into one of three categories. In the first category are the keyword cards that provide input to each of the multiphysics solvers that in turn couple with the structural solver. In the second category are keyword cards involving extensions to the basic solvers. Presently, the chemistry and stochastic particle solvers are the two solvers in this category, and they are used in conjunction with the compressible flow solver discussed below. In the third category are keyword cards for support facilities. A volume mesher that creates volume tetrahedral element meshes from bounding surface meshes is one of these tools. Another is a new data output mechanism for a limited set of variables from the solvers in this manual. This mechanism is accessed through *LSO keyword cards. The CESE solver is a compressible flow solver based upon the Conservation Ele- ment/Solution Element (CE/SE) method, originally proposed by Chang of the NASA Glenn Research Center. This method is a novel numerical framework for conservation laws. It has many non-traditional features, including a unified treatment of space and time, the introduction of separate conservation elements (CE) and solution elements (SE), and a novel shock capturing strategy without using a Riemann solver. This method has been used to solve many types of flow problems, such as detonation waves, shock/acoustic wave interaction, cavitating flows, supersonic liquid jets, and chemically reacting flows. In LS-DYNA, it has been extended to also solve fluid-structure interaction (FSI) problems. It does this with two approaches. The first approach solves the compressible flow equations on an Eulerian mesh while the structural mechanics is solved on a moving mesh that moves through the fixed CE/SE mesh. In the second approach (new with this version), the CE/SE mesh moves in a fashion such that its FSI boundary surface matches the corresponding FSI boundary surface of the moving structural mechanics mesh. This second approach is more accurate for FSI problems, especially with boundary layers flows. Another new feature with the CESE moving mesh solver is conjugate heat transfer coupling with the solid thermal solver. The chemistry and stochastic particle solvers are two addon solvers that extend the CESE solver. The second solver is the incompressible flow solver (ICFD) that is fully coupled with the solid mechanics solver. This coupling permits robust FSI analysis via either an explicit technique when the FSI is weak, or using an implicit coupling when the FSI coupling is strong. In addition to being able to handle free surface flows, there is also a bi-phasic flow capability that involves modeling using a conservative Lagrangian interface tracking technique. Basic turbulence models are also supported. This solver is the first in LS-DYNA to make use of a new volume mesher that takes surface meshes bounding the fluid domain as input (*MESH keywords). In addition, during the time advancement of the incompressible flow, the solution is adaptively re-meshed as an automatic feature of the solver. Another important feature of the mesher is the ability to create boundary layer meshes. These anisotropic meshes become a crucial part of the model when shear stresses are to be calculated near fluid walls. The ICFD solver is also coupled to the solid thermal solver using a monolithic approach for conjugate heat transfer problems. The third solver is an electromagnetics (EM) solver. This module solves the Maxwell equations in the Eddy current (induction-diffusion) approximation. This is suitable for cases where the propagation of electromagnetic waves in air (or vacuum) can be considered as instantaneous. Therefore, the wave propagation is not solved. The main applications are Magnetic Metal Forming, bending or welding, induced heating, ring expansions and so forth. The EM module allows the introduction of a source of electrical current into solid conductors and the computation of the associated magnetic field, electric field, as well as induced currents. The EM solver is coupled with the structural mechanics solver (the Lorentz forces are added to the mechanics equations of motion), and with the structural thermal solver (the ohmic heating is added to the thermal solver as an extra source of heat). The EM fields are solved using a Finite Element Method (FEM) for the conductors and a Boundary Element Method (BEM) for the surrounding air/insulators. Thus no air mesh is necessary. As stated above, the *CHEMISTRY and *STOCHASTIC cards are only used in the CESE solver at this time. *CESE The keyword *CESE provides input data for the Conservation Element/Solution Element (CESE) compressible fluid solver: *CESE_BOUNDARY_AXISYMMETRIC_{OPTION} *CESE_BOUNDARY_BLAST_LOAD *CESE_BOUNDARY_CONJ_HEAT_{OPTION} *CESE_BOUNDARY_CYCLIC_{OPTION} *CESE_BOUNDARY_FSI_{OPTION} *CESE_BOUNDARY_NON_REFLECTIVE_{OPTION} *CESE_BOUNDARY_PRESCRIBED_{OPTION} *CESE_BOUNDARY_REFLECTIVE_{OPTION} *CESE_BOUNDARY_SLIDING_{OPTION} *CESE_BOUNDARY_SOLID_WALL_{OPTION1}_{OPTION2} *CESE_CHEMISTRY_D3PLOT *CESE_CONTROL_LIMITER *CESE_CONTROL_MESH_MOV *CESE_CONTROL_SOLVER *CESE_CONTROL_TIMESTEP *CESE_DATABASE_ELOUT *CESE_DATABASE_FLUXAVG *CESE_DATABASE_FSIDRAG *CESE_DATABASE_POINTOUT *CESE_DATABASE_SSETDRAG *CESE_DEFINE_NONINERTIAL *CESE_DEFINE_POINT *CESE_EOS_CAV_HOMOG_EQUILIB *CESE *CESE_EOS_IDEAL_GAS *CESE_EOS_INFLATOR1 *CESE_EOS_INFLATOR2 *CESE_FSI_EXCLUDE *CESE_INITIAL *CESE_INITIAL_{OPTION} *CESE_INITIAL_CHEMISTRY *CESE_INITIAL_CHEMISTRY_ELEMENT *CESE_INITIAL_CHEMISTRY_PART *CESE_INITIAL_CHEMISTRY_SET *CESE_MAT_000 *CESE_MAT_001 (*CESE_MAT_GAS) *CESE_MAT_002 *CESE_PART *CESE_SURFACE_MECHSSID_D3PLOT *CESE_SURFACE_MECHVARS_D3PLOT Note that when performing a chemistry calculation with the CESE solver, initialization should only be done with the *CESE_INITIAL_CHEMISTRY_… cards, not the *CESE_INI- TIAL… cards. *CESE_BOUNDARY_AXISYMMETRIC_OPTION Available options are MSURF MSURF_SET SET SEGMENT Purpose: Define an axisymmetric boundary condition on the axisymmetric axis for the 2D axisymmetric CESE compressible flow solver. The MSURF and MSURF_SET options are used when the CESE mesh has been created using *MESH cards. The SET and SEGMENT cards are used when *ELEMENT_SOLID cards are used to define the CESE mesh. Surface Part Card. Card 1 format used when the MSURF keyword option is active. Provide as many cards as necessary. This input ends at the next keyword (“*”) card. Card 1a 1 2 3 4 5 6 7 8 Variable MSURFID Type I Default none Surface Part Set Card. Card 1 format used when the MSURF_SET keyword option is active. Provide as many cards as necessary. This input ends at the next keyword (“*”) card. Card 1b 1 2 3 4 5 6 7 8 Variable MSURF_S Type I Default none Set Card. Card 1 format used when the SET keyword option is active. Provide as many cards as necessary. This input ends at the next keyword (“*”) card. Card 1c 1 2 3 4 5 6 7 8 Variable SSID Type I Default none Segment Cards. Card 1 format used when SEGMENT keyword option is active. Include an additional card for each corresponding pair of segments. This input ends at the next keyword (“*”) card. Card 1d Variable 1 N1 2 N2 3 N3 4 N4 5 6 7 8 Type I I I I Default none none none none VARIABLE MSURFID MSURF_S DESCRIPTION Mesh surface part ID referenced in *MESH_SURFACE_ELEMENT cards. Identifier of a set of mesh surface part IDs created with a *LSO_ID_- SET card, where each mesh surface part ID in the set is referenced in *MESH_SURFACE_ELEMENT cards. SSID Segment set ID N1, N2, … Node IDs defining a segment Remarks: 1. This boundary condition can only be used on the axisymmetric axis for the 2D axisymmetric CESE fluid solver. *CESE_BOUNDARY_BLAST_LOAD_OPTION Available options include: MSURF MSURF_SET SET SEGMENT Purpose: For the CESE compressible flow solver, set boundary values for velocity, density, and pressure from a blast wave defined by a *LOAD_BLAST_ENHANCED card. Boundary values are applied at the centroid of elements connected with this boundary. OPTION = SET and OPTION = SEGMENT are for user defined meshes whereas OP- TION = MSURF or MSURF_SET are associated with the automatic volume mesher . That is, the MSURF and MSURF_SET options are used when the CESE mesh has been created using *MESH cards. The SET and SEGMENT cards are used when *ELEMENT_- SOLID cards are used to define the CESE mesh. Surface Part Card. Card 1 format used when the MSURF keyword option is active. Card 1a 1 2 3 4 5 6 7 8 Variable BID MSURFID Type I I Default none none Surface Part Set Card. Card 1 format used when the MSURF_SET keyword option is active. Card 1b 1 2 3 4 5 6 7 8 Variable BID MSURF_S Type I I Default none none Set Card. Card 1 format used when the SET keyword option is active. Card 1c 1 2 3 4 5 6 7 8 Variable BID SSID Type I I Default none none Segment Card. Card 1 for SEGMENT keyword option is active. Card 1d 1 Variable BID 2 N1 3 N2 4 N3 5 N4 6 7 8 Type I I I I I Default none none none none none VARIABLE DESCRIPTION BID Blast source ID . MSURFID MSURF_S A mesh surface part ID referenced in *MESH_SURFACE_ELEMENT cards Identifier of a set of mesh surface part IDs created with a *LSO_ID_- SET card, where each mesh surface part ID in the set is referenced in *MESH_SURFACE_ELEMENT cards. SSID Segment set ID N1, N2, … Node ID’s defining a segment *CESE_BOUNDARY_CONJ_HEAT_OPTION Available options are: MSURF MSURF_SET SET SEGMENT Purpose: Define a conjugate heat transfer interface condition for CESE compressible flows. This condition identifies those boundary faces of the CESE mesh that are in contact with non-moving structural parts, and through which heat flows. This is only possible when the structural thermal solver is also in being used in the structural parts. The MSURF and MSURF_SET options are used when the CESE mesh has been created using *MESH cards. The SET and SEGMENT cards are used when *ELEMENT_SOLID cards are used to define the CESE mesh. Surface Part Card. Card 1 used when the MSURF keyword option is active. Include as many cards as necessary. This input ends at the next keyword (“*”) card. Card 1a 1 2 3 4 5 6 7 8 Variable MSURFID Type I Default none Surface Part Set Card. Card 1 used when the MSURF_SET keyword option is active. Include as many cards as necessary. This input ends at the next keyword (“*”) card. Card 1b 1 2 3 4 5 6 7 8 Variable MSURF_S Type I Default none Set Card. Card 1 used when the SET keyword option is active. Include as many cards as necessary. This input ends at the next keyword (“*”) card. Card 1c 1 2 3 4 5 6 7 8 Variable SSID Type I Default none Segment Cards. Card 1 used when SEGMENT keyword option is active. Include an additional card for each corresponding pair of segments. This input ends at the next keyword (“*”) card. Card 1d Variable 1 N1 2 N2 3 N3 4 N4 5 6 7 8 Type I I I I Default none none none none VARIABLE MSURFID MSURF_S DESCRIPTION Mesh surface part ID referenced in *MESH_SURFACE_ELEMENT cards. Identifier of a set of mesh surface part IDs created with an *LSO_- ID_SET card, where each mesh surface part ID in the set is referenced in *MESH_SURFACE_ELEMENT cards. SSID Segment set ID N1, N2, … Node IDs defining a segment Remarks: 1. This boundary condition should only be imposed on a CESE mesh boundary that is in contact with non-moving structural parts. An Eulerian CESE solver is re- quired, as is use of the structural thermal solver. *CESE_BOUNDARY_CYCLIC_OPTION Available options are: MSURF MSURF_SET SET SEGMENT Purpose: Define a cyclic (periodic) boundary condition for CESE compressible flows. This cyclic boundary condition (CBC) can be used on periodic boundary surfaces. The MSURF and MSURF_SET options are used when the CESE mesh has been created using *MESH cards. The SET and SEGMENT cards are used when *ELEMENT_SOLID cards are used to define the CESE mesh. Card Sets. The following sequence of cards comprises a single set. LS-DYNA will continue reading *CESE_BOUNDARY_SOLID_WALL card sets until the next keyword (“*”) card is encountered. Surface Part Card. Card 1 format used when the MSURF keyword option is active. Card 1a 1 2 3 4 5 6 7 8 Variable MSURFID1 MSURFID2 CYCTYP Type I I Default none none Remarks I 0 1, 2 Surface Part Set Card. Card 1 format used when the MSURF_SET keyword option is active. Card 1b 1 2 3 4 5 6 7 8 Variable MSRF_S1 MSRF_S2 CYCTYP Type I I Default none none Remarks I 0 1, 3 Set Card. Card 1 format used when the SET keyword option is active. Card 1c 1 2 3 4 5 6 7 8 Variable SSID1 SSID2 CYCTYP Type I I Default none none Remarks I 0 1, 4 Segment Card. Card 1 format used when SEGMENT keyword option is active. Include an additional card for each corresponding pair of segments. This input ends at the next keyword (“*”) card. Card 1d 1 2 3 4 5 6 7 8 Variable ND1 ND2 ND3 ND4 NP1 NP2 NP3 NP4 Type I I I I I I I I Default none none none none none none none none Rotation Case Card. Additional card for the MSURF, MSURF_SET, and SET options when CYCTYP = 1. Card 2a 1 2 3 4 5 6 7 8 Variable AXISX1 AXISY1 AXISZ1 DIRX DIRY DIRZ ROTANG Type F F F F F F F Default 0.0 0.0 0.0 none none none none Translation Case Card. Additional card for the MSURF, MSURF_SET, and SET options when CYCTYP = 2. Card 2b 1 2 3 4 5 6 7 8 Variable TRANSX TRANSY TRANSZ Type F F F Default none none none VARIABLE DESCRIPTION MSURFID1, MSURFID2 Mesh surface part numbers referenced in *MESH_SURFACE_ELE- MENT cards. MSRF_S1, MSRF_S2 Identifiers of two sets of mesh surface part IDs, each created with a *LSO_ID_SET card, where each mesh surface part ID in each set is referenced in *MESH_SURFACE_ELEMENT cards. CYCTYP Relationship between the two cyclic boundary condition surfaces: EQ.0: none assumed (default) EQ.1: The first surface is rotated about an axis to match the second surface. EQ.2: The faces of the first surface are translated in a given direction to obtain the corresponding faces on the second surface. SSID1 & SSID2 A pair of segment set IDs *CESE_BOUNDARY_CYCLIC Node IDs defining a pair of segments: ND1, ND2, ND3, ND4 define the first segment, while NP1, NP2, NP3, NP4 define the second segment. This pair of segments must match either through a geometric translation or rotation. AXIS[Z,Y,Z]1 A point on the axis of rotation for CYCTYP.EQ.1. DIR[X,Y,Z] ROTANG The direction which together with AXIS[X,Y,Z]1 defines the axis of rotation for CYCTYP.EQ.1. The angle of rotation (in degrees) that transforms the centroid of each face on the first surface to the centroid of the corresponding face on the second surface (for CYCTYP.EQ.1). TRANS[X,Y,Z] The translation direction that enables the identification of the segment in the second surface that matches a segment in the first surface (for CYCTYP.EQ.2). Remarks: 1. For the MSURF, MSURF_SET, or SET options with CYCTYP.EQ.0, the code examines the geometry of two faces of the two surfaces in order to determine if the surfaces are approximately parallel (CYCTYP.EQ.2), or related through a rotation (CYCTYP.EQ.1). The geometric parameters required are then computed. 2. For the MSURF option, there must be the same number of mesh surface elements in each mesh surface part, and the mesh surface elements in each mesh surface part are then internally ordered in order to match pairwise between the two mesh surface parts. 3. For the MSURF_SET option, there must be the same number of mesh surface elements in each mesh surface part set, and the mesh surface elements in each mesh surface part set are then internally ordered in order to match pairwise be- tween the two mesh surface part sets. 4. For the SET option, there must be the same number of segments in each set, and the segments in each set are then internally ordered in order to match pairwise between the two sets. *CESE_BOUNDARY_FSI_OPTION Available options are: MSURF MSURF_SET SET SEGMENT Purpose: Define an FSI boundary condition for the moving mesh CESE compressible flow solver. This card must not be combined with the immersed-boundary method CESE solver, and doing so will result in an error termination condition. This boundary condition must be applied on a surface of the CESE computational domain that is co-located with surfaces of the outside boundary of the structural mechanics mesh. The nodes of the two meshes will generally not be shared. The MSURF and MSURF_SET options are used when the CESE mesh has been created using *MESH cards. The SET and SEGMENT cards are used when *ELEMENT_SOLID cards are used to define the CESE mesh. Surface Part Card. Card 1 format used when the MSURF keyword option is active. Provide as many cards as necessary. This input ends at the next keyword (“*”) card. Card 1a 1 2 3 4 5 6 7 8 Variable MSURFID Type I Default none Surface Part Set Card. Card 1 format used when the MSURF_SET keyword option is active. Provide as many cards as necessary. This input ends at the next keyword (“*”) card. Card 1b 1 2 3 4 5 6 7 8 Variable MSURF_S Type I Default none Set Card. Card 1 format used when the SET keyword option is active. Provide as many cards as necessary. This input ends at the next keyword (“*”) card. Card 1c 1 2 3 4 5 6 7 8 Variable SSID Type I Default none Segment Cards. Card 1 format used when SEGMENT keyword option is active. Include an additional card for each corresponding pair of segments. This input ends at the next keyword (“*”) card. Card 1d Variable 1 N1 2 N2 3 N3 4 N4 5 6 7 8 Type I I I I Default none none none none VARIABLE MSURFID DESCRIPTION Mesh surface part ID referenced in *MESH_SURFACE_ELEMENT cards. VARIABLE MSURF_S DESCRIPTION Identifier of a set of mesh surface part IDs created with a *LSO_ID_- SET card, where each mesh surface part ID in the set is referenced in *MESH_SURFACE_ELEMENT cards. SSID Segment set ID. N1, … Node IDs defining a segment Remarks: 1. This boundary condition card is also needed for conjugate heat transfer problems with the moving mesh CESE solver. *CESE_BOUNDARY_NON_REFLECTIVE_OPTION Available options are: MSURF MSURF_SET SET SEGMENT Purpose: Define a passive boundary condition for CESE compressible flows. This non- reflective boundary condition (NBC) provides an artificial computational boundary for an open boundary that is passive. The MSURF and MSURF_SET options are used when the CESE mesh has been created using *MESH cards. The SET and SEGMENT cards are used when *ELEMENT_SOLID cards are used to define the CESE mesh. Surface Part Card. Card 1 used when the MSURF keyword option is active. Include as many cards as necessary. This input ends at the next keyword (“*”) card. Card 1a 1 2 3 4 5 6 7 8 Variable MSURFID Type I Default none Surface Part Set Card. Card 1 used when the MSURF_SET keyword option is active. Include as many cards as necessary. This input ends at the next keyword (“*”) card. Card 1b 1 2 3 4 5 6 7 8 Variable MSURF_S Type I Default none Set Card. Card 1 used when the SET keyword option is active. Include as many cards as necessary. This input ends at the next keyword (“*”) card. Card 1c 1 2 3 4 5 6 7 8 Variable SSID Type I Default none Segment Cards. Card 1 used when SEGMENT keyword option is active. Include an additional card for each corresponding pair of segments. This input ends at the next keyword (“*”) card. Card 1d Variable 1 N1 2 N2 3 N3 4 N4 5 6 7 8 Type I I I I Default none none none none VARIABLE MSURFID MSURF_S DESCRIPTION Mesh surface part ID referenced in *MESH_SURFACE_ELEMENT cards. Identifier of a set of mesh surface part IDs created with an *LSO_- ID_SET card, where each mesh surface part ID in the set is referenced in *MESH_SURFACE_ELEMENT cards. SSID Segment set ID N1, N2, … Node IDs defining a segment Remarks: 1. This boundary condition is usually imposed on an open surface that is far from the main disturbed flow (the further away, the better), i.e., the flow on that boundary surface should be almost uniform. 2. If any boundary segment has not been assigned a boundary condition by any of the *CESE_BOUNDARY_… cards, then it will automatically be assigned this non- reflective boundary condition. *CESE_BOUNDARY_PRESCRIBED_OPTION Available options include: MSURF MSURF_SET SET SEGMENT Purpose: For the CESE compressible flow solver, set boundary values for velocity, density, pressure and temperature. Boundary values are applied at the centroid of elements connected with this boundary. OPTION = SET and OPTION = SEGMENT are for user defined meshes whereas OPTION = MSURF or MSURF_SET are associated with the automatic volume mesher . That is, the MSURF and MSURF_SET options are used when the CESE mesh has been created using *MESH cards. The SET and SEGMENT cards are used when *ELEMENT_SOLID cards are used to define the CESE mesh. Card Sets: A set of data cards for this keyword consists of 3 of the following cards: 1. Card 1 specifies the object to which the boundary condition is applied. Its format depends on the keyword option. 2. Card 2 reads in load curve IDs. 3. Card 3 reads in scale factors. For each boundary condition to be specified include one set of cards. This input ends at the next keyword (“*”) card. Surface Part Card. Card 1 format used when the MSURF keyword option is active. Card 1a 1 2 3 4 5 6 7 8 Variable MSURFID IDCOMP Type I I Default none none Surface Part Set Card. Card 1 format used when the MSURF_SET keyword option is active. Card 1b 1 2 3 4 5 6 7 8 Variable MSURF_S IDCOMP Type I I Default none none Set Card. Card 1 format used when the SET keyword option is active. Card 1c 1 2 3 4 5 6 7 8 Variable SSID IDCOMP Type I I Default none none Segment Card. Card 1 for SEGMENT keyword option is active. Card 1d Variable 1 N1 2 N1 3 N3 4 N4 5 6 7 8 IDCOMP Type I I I I I Default none none none none none Load Curve Card. Card 2 1 2 3 4 5 6 7 8 Variable LC_U LC_V LC_W LC_RHO LC_P LC_T Type I I I I I I Remarks 1,2,3 1,2,3 1,2,3 1,2,3 1,2,3 1,2,3 Scale Factor Card. Card 3 1 2 3 4 5 6 7 8 Variable SF_U SF_V SF_W SF_RHO SF_P SF_T Type F F F F F F Default 1.0 1.0 1.0 1.0 1.0 1.0 Remarks 2 2 2 2 2 2 VARIABLE MSURFID MSURF_S DESCRIPTION A mesh surface part ID referenced in *MESH_SURFACE_ELEMENT cards Identifier of a set of mesh surface part IDs created with a *LSO_ID_- SET card, where each mesh surface part ID in the set is referenced in *MESH_SURFACE_ELEMENT cards. SSID Segment set ID N1, N2, … Node ID’s defining a segment IDCOMP For inflow boundaries in problems involving chemical reacting flows, the chemical mixture of the fluid entering the domain is defined with a *CHEMISTRY_COMPOSITION card with this ID. LC_U Load curve ID to describe the x-component of the velocity versus time; see *DEFINE_CURVE. LC_V LC_W *CESE_BOUNDARY_PRESCRIBED DESCRIPTION Load curve ID to describe the y-component of the velocity versus time. Load curve ID to describe the z-component of the velocity versus time. LC_RHO Load curve ID to describe the density versus time. LC_P LC_T SF_U SF_V Load curve ID to describe the pressure versus time. Load curve ID to describe the temperature versus time. Scale factor for LC_U (default = 1.0). Scale factor for LC_V (default = 1.0). SF_W Scale factor for LC_W (default = 1.0). SF_RHO Scale factor for LC_RHO (default = 1.0). Scale factor for LC_P (default = 1.0). Scale factor for LC_T (default = 1.0). SF_P SF_T Remarks: 1. On each centroid or set of centroids, the variables (𝑣𝑥, 𝑣𝑦, 𝑣𝑧, 𝜌, 𝑃, 𝑇) that are given values must be consistent and make the model well-posed (i.e., be such that the solution of the model exists, is unique and physical). 2. 3. If any of the load curves are 0, the corresponding variable will take the constant value of the corresponding scale factor. For instance, if LC_RHO = 0, then the constant value of the density for this boundary condition will be SF_RHO. If a load ID is -1 for a given variable, then the boundary value for that variable is computed by the solver, and not specified by the user. *CESE_BOUNDARY_REFLECTIVE_OPTION Available options are: MSURF MSURF_SET SET SEGMENT Purpose: Define a reflective boundary condition (RBC) for the CESE compressible flow solver. This boundary condition can be applied on a symmetrical surface or a solid wall of the computational domain. The MSURF and MSURF_SET options are used when the CESE mesh has been created using *MESH cards. The SET and SEGMENT cards are used when *ELEMENT_SOLID cards are used to define the CESE mesh. Surface Part Card. Card 1 format used when the MSURF keyword option is active. Provide as many cards as necessary. This input ends at the next keyword (“*”) card. Card 1a 1 2 3 4 5 6 7 8 Variable MSURFID Type I Default none Surface Part Set Card. Card 1 format used when the MSURF_SET keyword option is active. Provide as many cards as necessary. This input ends at the next keyword (“*”) card. Card 1b 1 2 3 4 5 6 7 8 Variable MSURF_S Type I Default none Set Card. Card 1 format used when the SET keyword option is active. Provide as many cards as necessary. This input ends at the next keyword (“*”) card. Card 1c 1 2 3 4 5 6 7 8 Variable SSID Type I Default none Segment Cards. Card 1 format used when SEGMENT keyword option is active. Include an additional card for each corresponding pair of segments. This input ends at the next keyword (“*”) card. Card 1d Variable 1 N1 2 N2 3 N3 4 N4 5 6 7 8 Type I I I I Default none none none none VARIABLE MSURFID MSURF_S DESCRIPTION Mesh surface part ID referenced in *MESH_SURFACE_ELEMENT cards. Identifier of a set of mesh surface part IDs created with a *LSO_ID_- SET card, where each mesh surface part ID in the set is referenced in *MESH_SURFACE_ELEMENT cards. SSID Segment set ID. N1, N2, … Node IDs defining a segment Remarks: 1. This boundary condition has the same effect as a solid-wall boundary condition for inviscid flows. *CESE_BOUNDARY_SLIDING_OPTION Available options are: MSURF MSURF_SET SET SEGMENT Purpose: Allows nodes of a fluid surface to translate in the main direction of mesh movement. This is useful in piston type applications. The MSURF and MSURF_SET options are used when the CESE mesh has been created using *MESH cards. The SET and SEGMENT cards are used when *ELEMENT_SOLID cards are used to define the CESE mesh. Surface Part Card. Card 1 format used when the MSURF keyword option is active. Provide as many cards as necessary. This input ends at the next keyword (“*”) card. Card 1a 1 2 3 4 5 6 7 8 Variable MSURFID Type I Default none Surface Part Set Card. Card 1 format used when the MSURF_SET keyword option is active. Provide as many cards as necessary. This input ends at the next keyword (“*”) card. Card 1b 1 2 3 4 5 6 7 8 Variable MSURF_S Type I Default none Set Card. Card 1 format used when the SET keyword option is active. Provide as many cards as necessary. This input ends at the next keyword (“*”) card. Card 1c 1 2 3 4 5 6 7 8 Variable SSID Type I Default none Segment Cards. Card 1 format used when SEGMENT keyword option is active. Include an additional card for each corresponding pair of segments. This input ends at the next keyword (“*”) card. Card 1d Variable 1 N1 2 N2 3 N3 4 N4 5 6 7 8 Type I I I I Default none none none none VARIABLE MSURFID MSURF_S DESCRIPTION Mesh surface part ID referenced in *MESH_SURFACE_ELEMENT cards. Identifier of a set of mesh surface part IDs created with a *LSO_ID_- SET card, where each mesh surface part ID in the set is referenced in *MESH_SURFACE_ELEMENT cards. SSID Segment set ID N1, N2, … Node IDs defining a segment *CESE_BOUNDARY_SOLID_WALL_OPTION1_OPTION2 For OPTION1 the choices are: MSURF MSURF_SET SET SEGMENT For OPTION2 the choices are: <BLANK> ROTAT Purpose: Define a solid wall boundary condition (SBC) for this CESE compressible flow solver. This boundary condition can be applied at a solid boundary that is the physical boundary for the flow field. For inviscid flow, this will be a slip boundary condition; while for viscous flows, it is a no-slip boundary condition. The MSURF and MSURF_SET options are used when the CESE mesh has been created using *MESH cards. The SET and SEGMENT cards are used when *ELEMENT_SOLID cards are used to define the CESE mesh. Card Sets. The following sequence of cards comprises a single set. LS-DYNA will continue reading *CESE_BOUNDARY_SOLID_WALL card sets until the next keyword (“*”) card is encountered. Surface Part Card. Card 1 format used when the MSURF keyword option is active. Card 1a 1 2 Variable MSURFID LCID Type I Default none I 0 3 Vx F 4 Vy F 5 Vz F 6 Nx F 7 Ny F 8 Nz F 0.0 0.0 0.0 0.0 0.0 0.0 Remarks 2, 3 2 2 2 3 3 Surface Part Set Card. Card 1 format used when the MSURF_SET keyword option is active. Card 1b 1 2 Variable MSURF_S LCID Type I Default none I 0 3 Vx F 4 Vy F 5 Vz F 6 Nx F 7 Ny F 8 Nz F 0.0 0.0 0.0 0.0 0.0 0.0 Remarks 2, 3 2 2 2 3 3 3 Set Card. Card 1 format used when the SET keyword option is active. Card 1c 1 2 Variable SSID LCID Type I Default none I 0 3 Vx F 4 Vy F 5 Vz F 6 Nx F 7 Ny F 8 Nz F 0.0 0.0 0.0 0.0 0.0 0.0 Remarks 2, 3 2 2 2 3 3 3 Segment Card. Card 1 format used when SEGMENT keyword option is active. Card 1d Variable 1 N1 2 N2 3 N3 4 N4 5 LCID Type I I I I Default none none none none I 0 6 Vx F 7 Vy F 8 Vz F 0.0 0.0 0.0 Remarks 2, 3 2 2 Rotating Axis Card. Additional card read when the ROTAT keyword option is set. 4 5 6 7 8 Card 2 Variable 1 Nx Type F 2 Ny F 3 Nz F Default 0.0 0.0 0.0 Remarks 3 3 3 VARIABLE MSURFID MSURF_S DESCRIPTION Mesh surface part ID referenced in *MESH_SURFACE_ELEMENT cards. Identifier of a set of mesh surface part IDs created with a *LSO_ID_- SET card, where each mesh surface part ID in the set is referenced in *MESH_SURFACE_ELEMENT cards. SSID Segment set ID N1, N2, … Node ID’s defining a segment LCID Load curve ID to define this solid wall boundary movement If OPTION2 = <BLANK>: Vx, Vy, Vz velocity vector of the solid wall: LCID.EQ.0: it is defined by (Vx, Vy, Vz) itself; LCID.NE.0: it will be defined by both of the load curve and (Vx, Vy, Vz); Nx, Ny, Nz are not used in this case. If OPTION2 = ROTAT: Vx, Vy, Vz x-,y- & z-coordinates of a point on the rotating axis Nx, Ny, Nz Unit vector of the rotating axis (for the 2D case, this is not used). The rotating frequency (Hz) is given by the load curve. *CESE_BOUNDARY_SOLID_WALL 1. In this solid-wall condition (SBC), the boundary movement can only be in the tangential direction of the wall and should not affect the fluid domain size and mesh during the calculation, otherwise an FSI or moving mesh solver should be used. Also, this moving SBC only affects viscous flows (no-slip BC). 2. If LCID = 0 and Vx = Vy = Vz = 0.0 (default), this will be a regular solid wall BC. 3. For rotating SBC, LCID > 0 must be used to define the rotating speed frequency (Hz). Also, in the 2D case, (Nx, Ny, Nz) does not need to be defined because it is not needed. *CESE Purpose: Cause mass fractions of the listed chemical species to be added to the CESE d3plot output. This is only used when chemistry is being solved with the CESE solver. Card 1 1 2 3 4 5 6 7 8 Variable MODELID Type I Default none Species Cards. Include one card for each species to be included in the d3plot database. This input ends at the next keyword (“*”) card. Card 2 1 2 3 4 5 6 7 8 Variable Type SPECIES A VARIABLE DESCRIPTION MODELID Identifier of a Chemkin-compatible chemistry model. SPECIES Name of a chemical species that is defined in the chemistry model identified by MODELID . *CESE_CONTROL_LIMITER Purpose: Sets some stability parameters used in the CESE scheme for this CESE compressible flow solver. Card 1 1 2 3 4 5 6 7 8 Variable IDLMT ALFA BETA EPSR Type Default I 0 F F F 0.0 0.0 0.0 Remarks 1 2 3 VARIABLE DESCRIPTION IDLMT Set the stability limiter option : EQ.0: limiter format 1 (Re-weighting). EQ.1: limiter format 2 (Relaxing). Re-weighting coefficient Numerical viscosity control coefficient Stability control coefficient ALFA BETA EPSR Remarks: 1. 𝛼 ≥ 0; larger values give more stability, but less accuracy. Usually α = 2.0 or 4.0 will be enough for normal shock problems. 2. 3. 0 ≤ 𝛽 ≤ 1; larger values give more stability. For problems with shock waves, β = 1.0 is recommended. 𝜀 ≥ 0; larger values give more stability, but less accuracy. *CESE Purpose: For moving mesh CESE, this keyword is used to choose the type of algorithm to be used for calculating mesh movement. Card 1 1 2 3 4 5 6 7 8 Variable MMSH LIM_ITER RELTOL Type Default I 1 I F 100 1.0e-3 VARIABLE DESCRIPTION MMSH Mesh motion selector: EQ.1: mesh moves using an implicit ball-vertex spring method. EQ.9: the IDW scheme is used to move the mesh. Maximum number of linear solver iterations for the implicit ball- vertex spring linear system. Relative tolerance to use as a stopping criterion for the iterative linear solver (conjugate gradient solver with diagonal scaling preconditioner). LIM_ITER RELTOL . *CESE_CONTROL_SOLVER Purpose: Set general purpose control variables for the CESE compressible flow solver. Card 1 1 2 3 4 5 6 7 8 Variable ICESE IFLOW IGEOM IFRAME MIXID IDC ISNAN Type Default I 0 I 0 Remarks I none 1, 2 I 0 I F none 0.25 I 0 3 VARIABLE DESCRIPTION ICESE Sets the framework of the CESE solver. EQ.0: Fixed Eulerian EQ.100: Moving Mesh FSI EQ.200: Immersed boundary FSI IFLOW Sets the compressible flow types: EQ.0: Viscous flows (laminar) EQ.1: Invisid flows IGEOM Sets the geometric dimension: EQ.2: Two-dimensional (2D) problem EQ.3: Three-dimensional (3D) problem EQ.101: 2D axisymmetric IFRAME Choose the frame of reference: EQ.0: Usual non-moving reference frame (default). EQ.1000: Non-inertial rotating reference frame. MIXID Chemistry model ID that defines the chemical species to include in the mixing model . The species information is given through the model’s card specifying the Chemkin-compatible input. VARIABLE DESCRIPTION Contact interaction detection coefficient (for FSI and conjugate heat transfer problems). Flag to check for a NaN in the CESE solver solution arrays at the completion of each time step. This option can be useful for debugging purposes. There is a cost overhead when this option is active. EQ.0: No checking, EQ.1: Checking is active. IDC ISNAN Remarks: 1. If the user wants to use the 2D (IGEOM = 2) or 2D axisymmetric (IGEOM = 101) solver, the mesh should only be distributed in the x-y plane with the boundary conditions given only at the 𝑥-𝑦 domain boundaries. Otherwise, a warning mes- sage will be given and the 3D solver will be triggered instead. 2. The 2D axisymmetric case will work only if the 2D mesh and corresponding boundary conditions are properly defined, with the 𝑥 and 𝑦 coordinates corre- sponding to the radial and axial directions respectively. 3. IDC is the same type of variable that is input on the *ICFD_CONTROL_FSI card. For an explanation, see Remark 1 for the *ICFD_CONTROL_FSI card. *CESE_CONTROL_TIMESTEP Purpose: Sets the time-step control parameters for the CESE compressible flow solver. Card 1 1 2 3 4 5 6 7 8 Variable IDDT CFL DTINT Type Default I 0 F F 0.9 1.0E-3 VARIABLE DESCRIPTION IDDT Sets the time step option: EQ.0: Fixed time step size (DTINT, i.e., given initial time step size) NE.0: the time step size will be calculated based on the given CFL-number and the flow solution at the previous time step. CFL CFL number (Courant–Friedrichs–Lewy condition) ( 0.0 < CFL ≤ 1.0 ) DTINT Initial time step size *CESE Purpose: This keyword enables the output of CESE data on elements. If more than one element set is defined, then several output files will be generated. Output Options Card. Card 1 1 2 3 4 5 6 7 8 Variable OUTLV DTOUT Type Default I 0 F 0. Include as many cards as needed. This input ends at the next keyword (“*”) card. Card 2 1 2 3 4 5 6 7 8 Variable ELSID Type I Default none VARIABLE DESCRIPTION OUTLV Determines if the output file should be dumped. EQ.0: No output file is generated. EQ.1: The output file is generated. DTOUT Time interval to print the output. If DTOUT is equal to 0.0, then the CESE timestep will be used. ELSID Solid Elements Set ID. Remarks: 1. The file name for this database is cese_elout.dat. *CESE_CONTROL_TIMESTEP Purpose: This keyword enables the output of CESE data on segment sets. If more than one segment set is defined, then several output files will be generated. Output Options Card. Card 1 1 2 3 4 5 6 7 8 Variable OUTLV DTOUT Type Default I 0 F 0. Include as many cards as needed. This input ends at the next keyword (“*”) card. Card 2 1 2 3 4 5 6 7 8 Variable SSID Type I Default none VARIABLE DESCRIPTION OUTLV Determines if the output file should be dumped. EQ.0: No output file is generated. EQ.1: The output file giving the average fluxes is generated. DTOUT Time interval to print the output. If DTOUT is equal to 0.0, then the CESE timestep will be used. SSID Segment Set ID. Remarks: 1. The file names for this database is cese_fluxavg.dat. *CESE Purpose: This keyword enables the output of the total fluid pressure force applied on solid parts in FSI problems at every time step. Output Options Card. Card 1 1 2 3 4 5 6 7 8 Variable OUTLV Type Default I 0 VARIABLE DESCRIPTION OUTLV Determines if the output file should be dumped. EQ.0: No output file is generated. EQ.1: The output file giving the pressure forces is generated. Remarks: 1. The file names for this database are cese_dragsol.dat, cese_dragshell.dat, cese_dragsol2D.dat and cese_dragbeam.dat .depending on what kind of solid is used. *CESE_CONTROL_TIMESTEP Purpose: This keyword enables the output of CESE data on points. Output Options Card. Card 1 1 2 3 Variable PSID DTOUT PSTYPE Type Default I 0 F 0. I 0 4 VX F 0. 5 VY F 0. 6 VZ F 0. 7 8 Include as many cards as needed. This input ends at the next keyword (“*”) card. 5 6 7 8 Card 2 1 Variable PID Type I 2 X F 3 Y F 4 Z F Default none none none none VARIABLE DESCRIPTION PSID Point Set ID. DTOUT Time interval to print the output. If DTOUT is equal to 0.0, then the CESE timestep will be used. PSTYPE Point Set type : EQ.0: Fixed points. EQ.1: Tracer points using prescribed velocity. EQ.2: Tracer points using fluid velocity. VX, VY, VZ Constant velocities to be used when PSTYPE = 1 PID Point ID X, Y, Z Point initial coordinates Remarks: 1. The file name for this database is cese_pointout.dat. *CESE_DATABASE_SSETDRAG Purpose: This keyword enables the output of CESE drag forces on segment sets. If more than one segment set is defined, then several output files will be generated. Output Options Card. Card 1 1 2 3 4 5 6 7 8 Variable OUTLV DTOUT Type Default I 0 F 0. Include as many cards as needed. This input ends at the next keyword (“*”) card. Card 2 1 2 3 4 5 6 7 8 Variable SSID Type I Default none VARIABLE DESCRIPTION OUTLV Determines if the output file should be dumped. EQ.0: No output file is generated. EQ.1: The output file giving the average fluxes is generated. DTOUT Time interval to print the output. If DTOUT is equal to 0.0, then the CESE timestep will be used. SSID Segment Set ID. Remarks: 1. The file name for this database is cese_ssetdrag.dat. 2. In order for the friction drag to give consistent results, special care must be given to the mesh close to the solid wall boundary (Good capturing of the boundary layer behavior). A very fine structured mesh is recommended. *CESE_DEFINE_NONINERTIAL Purpose: Define the CESE problem domain as a non-inertial rotating frame that rotates at a constant rate. This is used in rotating problems such as spinning cylinders, wind turbines and turbo machinery. Card 1 1 2 Variable FREQ LCID Type F Default none Card 2 Variable Type 1 L F I 0 2 R F Default none none 7 8 3 PID I 4 Nx F 5 Ny F 6 Nz F none none none none 3 4 5 6 7 8 RELV I 0 VARIABLE DESCRIPTION FREQ LCID PID Frequency of rotation. Load curve ID for scaling factor of FREQ. Starting point ID for the reference frame . Nx, Ny, Nz Rotating axis direction. L R Length of rotating frame. Radius of rotating frame. VARIABLE DESCRIPTION RELV Velocity display mode: EQ.0: Relative velocity, only the non-rotating components of the velocity are output. EQ.1: Absolute velocity is output. *CESE_POINT Purpose: Define points to be used by the CESE solver. Point Cards. Include one card for each point. This input ends at the next keyword (“*”) card. 5 6 7 8 Card 1 1 Variable NID Type I 2 X F 3 Y F 4 Z F Default none none none none VARIABLE DESCRIPTION NID Identifier for this point. X, Y, Z Coordinates of the point. *CESE Purpose: Provide the far-field (or free-stream) fluid pressure. Card 1 1 2 3 4 5 6 7 8 Variable PRESS Type F VARIABLE PRESS DESCRIPTION Value of the free-stream fluid pressure (in units used by the current problem). *CESE_EOS_CAV_HOMOG_EQUILIB Purpose: Define the coefficients in the equation of state (EOS) for the homogeneous equilibrium cavitation model. Include as many cards as needed. This input ends at the next keyword (“*”) card. Card 1 1 Variable EOSID 2 vap 3 liq 4 𝑎vap 5 𝑎liq 6 vap 7 liq 8 𝑃SatVap Type I F F F F F F Default none 0.8 880.0 334.0 1386.0 1.435e- 5 1.586e- 4 1.2e+4 VARIABLE DESCRIPTION EOSID Equation of state identifier vap liq 𝑎vap 𝑎liq vap liq density of the saturated vapor density of the saturated liquid sound speed of the saturated vapor sound speed of the saturated liquid dynamic viscosity of the vapor dynamic viscosity of the liquid 𝑃SatVap pressure of the saturated vapor Remarks: 1. Once a cavitation EOS is used, the cavitation flow solver will be triggered. 2. In this homogeneous equilibrium cavitation model, a barotropic equation of state is used. This model can be used in small scale & high speed cavitation flows, and it is not good for large-scale, low-speed cavitation calculations. *CESE Purpose: Define the coefficients Cv and Cp in the equation of state for an ideal gas in the CESE fluid solver. 4 5 6 7 8 Card 1 1 Variable EOSID Type I 2 Cv F 3 Cp F Default none 717.5 1004.5 VARIABLE DESCRIPTION EOSID Equation of state identifier Cv Cp Specific heat at constant volume Specific heat at constant pressure Remarks: 1. As with other solvers in LS-DYNA, the user is responsible for unit consistency. For example, if a user wants to use dimensionless variables, Cv & Cp above also should be replaced by the corresponding dimensionless ones. *CESE_EOS_INFLATOR1 Purpose: To define an EOS using Cp and Cv thermodynamic expansions for an inflator gas mixture with a single temperature range. Card 1 1 2 3 4 5 6 7 8 Variable EOSID Type I Default none Card 2 1 2 3 4 5 6 7 8 Variable Cp0 Cp1 Cp2 Cp3 Cp4 Type F Default 0. F 0. F 0. F 0. F 0. Card 3 1 2 3 4 5 6 7 8 Variable Cv0 Cv1 Cv2 Cv3 Cv4 Type F Default 0. F 0. F 0. F 0. F 0. VARIABLE DESCRIPTION EOSID Equation of state identifier for the CESE solver. Cp0, …, Cp4 Coefficients of temperature-dependent specific heat at constant pressure Cp(T) = Cp0 + Cp1 T + Cp2 T2 + Cp3 T3 + Cp4 T4 DESCRIPTION Coefficients of temperature-dependent specific heat at constant volume Cv(T) = Cv0 + Cv1 T + Cv2 T2 + Cv3 T3 + Cv4 T4 VARIABLE Cv0, …, Cv4 Remark: 1.These coefficient expansions for the specific heats over the entire temperature range are See and *CHEMISTRY_CONTROL_INFLATOR *CHEMISTRY_INFLATOR_PROPERTIES for details related to running that solver. inflator model generated solver. 0-D the by *CESE_EOS_INFLATOR2 Purpose: To define an EOS using Cp and Cv thermodynamic expansions for an inflator gas mixture with two temperature ranges, one below 1000 degrees Kelvin, and the other above 1000 degrees Kelvin. Card 1 1 2 3 4 5 6 7 8 Variable EOSID Type I Default none Card for the expansion of Specific Heat at Constant Pressure. Valid for T < 1000 0 K Card 2 1 2 3 4 5 6 7 8 Variable Cp1_0 Cp1_1 Cp1_2 Cp1_3 Cp1_4 Type F Default 0. F 0. F 0. F 0. F 0. Card for the expansion of Specific Heat at Constant Pressure. Valid for T > 1000 0 K. Card 3 1 2 3 4 5 6 7 8 Variable Cp2_0 Cp2_1 Cp2_2 Cp2_3 Cp2_4 Type F Default 0. F 0. F 0. F 0. F 0. Card for the expansion of Specific Heat at Constant Volume. Valid for T < 1000 0 K Card 4 1 2 3 4 5 6 7 8 Variable Cv1_0 Cv1_1 Cv1_2 Cv1_3 Cv1_4 Type F Default 0. F 0. F 0. F 0. F 0. Card for the expansion of Specific Heat at Constant Volume. Valid for T > 1000 0 K. Card 5 1 2 3 4 5 6 7 8 Variable Cv2_0 Cv2_1 Cv2_2 Cv2_3 Cv2_4 Type F Default 0. F 0. F 0. F 0. F 0. VARIABLE DESCRIPTION EOSID Equation of state identifier for the CESE solver. Cp1_0, …, Cp1_4 Coefficients of temperature-dependent specific heat at constant pressure valid for T < 1000 0 K. Cp1(T) = Cp1_0 + Cp1_1 T + Cp1_2 T2 + Cp1_3 T3 + Cp1_4 T4 Cp2_0, …, Cp2_4 Coefficients of temperature-dependent specific heat at constant pressure valid for T > 1000 0 K. Cp2(T) = Cp2_0 + Cp2_1 T + Cp2_2 T2 + Cp2_3 T3 + Cp2_4 T4 Cv1_0, …, Cv1_4 Coefficients of temperature-dependent specific heat at constant volume valid for T < 1000 0 K. Cv1(T) = Cv1_0 + Cv1_1 T + Cv1_2 T2 + Cv1_3 T3 + Cv1_4 T4 Cv2_0, …, Cv2_4 Coefficients of temperature-dependent specific heat at constant volume valid for T > 1000 0 K. Cv2(T) = Cv2_0 + Cv2_1 T + Cv2_2 T2 + Cv2_3 T3 + Cv2_4 T4 *CESE_EOS_INFLATOR2 2.These coefficient expansions for the specific heats over two temperature ranges are See generated *CHEMISTRY_CONTROL_INFLATOR and *CHEMISTRY_INFLATOR_PROPERTIES for details related to running that solver. inflator solver. model 0-D the by *CESE Purpose: Provide a list of mechanics solver parts that are not involve in the CESE FSI calculation. This is intended to be used as an efficiency measure for parts that will not involve significant FSI interactions with the CESE compressible fluid solver.. Include as many cards as needed. This input ends at the next keyword (“*”) card. Card 1 1 2 3 4 5 6 7 8 Variable PID1 PID2 PID3 PID4 PID5 PID6 PID7 PID8 Type I I I I I I I I Default none none none none none none none none VARIABLE PIDn DESCRIPTION IDs of mechanics parts that will be excluded from the FSI interaction calculation with the CESE solver. *CESE_INITIAL Purpose: Specify constant initial conditions (ICs) for flow variables at the centroid of each fluid element. Card 1 Variable Type Default 1 U F 0 2 V F 3 W F 4 RH F 5 P F 6 T F 0.0 0.0 1.225 0.0 0.0 7 8 VARIABLE DESCRIPTION U, V, W x-, y-, z-velocity components respectively density ρ pressure Ρ temperature Τ RHO P T Remarks: 1. Usually, only two of ρ, Ρ & Τ are needed to be specified (besides the velocity). If all three are given, only ρ and Ρ will be used. 2. These initial condition will be applied in those elements that have not been assigned a value by *CESE_INITIAL_OPTION cards for individual elements or sets of elements. *CESE_INITIAL_{OPTION} *CESE_INITIAL_{OPTION} Available options include: SET ELEMENT *CESE Purpose: Specify initial conditions for the flow variables at the centroid of each element in a set of elements or at the centroid of a single element. Include as many cards as needed. This input ends at the next keyword (“*”) card. Card 1 1 Variable EID/ESID Type I 2 U F 3 V F 4 W F 5 RHO F 6 P F 7 T F 8 Default none 0.0 0.0 0.0 1.225 0.0 0.0 Remarks 1 1 1 VARIABLE DESCRIPTION EID/ESID Solid element ID (EID) or solid element set ID (ESID) U, V, W x-, y-, z-velocity components respectively RHO density P T pressure temperature Remarks: 1. Usually, only two of ρ, Ρ & Τ are needed to be specified (besides the velocity). If all three are given, only ρ and Ρ will be used. 2. The priority of this card is higher than *CESE_INITIAL, i.e., if an element is assigned an initial value by this card, *CESE_INITIAL will no longer apply to that element. *CESE_INITIAL_CHEMISTRY Purpose: Initializes the chemistry and fluid state in every element of the CESE mesh that has not already been initialized by one of the other *CESE_INITIAL_CHEMISTRY cards. This is only used when chemistry is being solved with the CESE solver. Card 1 1 2 3 4 5 6 7 8 Variable CHEMID COMPID Type I I Default none none Card 2 1 Variable UIC 2 VIC 3 4 5 WIC RHOIC PIC 6 TIC 7 HIC 8 Type F F F F F F F Default none none none none none none none VARIABLE DESCRIPTION CHEMID Identifier of chemistry control card to use. COMPID Identifier of chemical composition to use. UIC VIC WIC X-component of the fluid velocity. Y-component of the fluid velocity. Z-component of the fluid velocity. RHOIC Initial fluid density. PIC TIC Initial fluid pressure. Initial fluid temperature. VARIABLE HIC DESCRIPTION Initial fluid enthalpy. However, when CHEMID refers to a ZND 1- step reaction card, this is the progressive variable (degree of combustion). *CESE_INITIAL_CHEMISTRY_ELEMENT Purpose: Initializes the chemistry and fluid state in every element of the list of CESE elements. This is only used when chemistry is being solved with the CESE solver. Card 1 1 2 3 4 5 6 7 8 Variable CHEMID COMPID Type I I Default none none Card 2 1 Variable UIC 2 VIC 3 4 5 WIC RHOIC PIC 6 TIC 7 HIC 8 Type F F F F F F F Default none none none none none none none Element List Card. Provide as many cards as necessary. This input ends at the next keyword (“*”) card. Card 3 1 2 3 4 5 6 7 8 Variable ELE1 ELE2 ELE3 ELE4 ELE5 ELE6 ELE7 ELE8 Type I I I I I I I I Default none none none none none none none none VARIABLE DESCRIPTION CHEMID Identifier of chemistry control card to use. COMPID Identifier of chemical composition to use. VARIABLE DESCRIPTION UIC VIC WIC X-component of the fluid velocity. Y-component of the fluid velocity. Z-component of the fluid velocity. RHOIC Initial fluid density. PIC TIC HIC Initial fluid pressure. Initial fluid temperature. Initial fluid enthalpy. However, when CHEMID refers to a ZND 1- step reaction card, this is the progressive variable (degree of combustion). ELE1, … User element numbers to initialize. *CESE_INITIAL_CHEMISTRY_PART Purpose: Initializes the chemistry and fluid state in every element of the specified CESE part that has not already been initialized by *CESE_INITIAL_CHEMISTRY_ELEMENT or *CESE_INITIAL_CHEMISTRY_SET cards. This is only used when chemistry is being solved with the CESE solver. Card 1 1 2 3 4 5 6 7 8 Variable PARTID CHEMID COMPID Type I I I Default none none none Card 2 1 Variable UIC 2 VIC 3 4 5 WIC RHOIC PIC 6 TIC 7 HIC 8 Type F F F F F F F Default none none none none none none none VARIABLE DESCRIPTION PARTID Identifier of the CESE part on which to initialize. CHEMID Identifier of chemistry control card to use. COMPID Identifier of chemical composition to use. UIC VIC WIC X-component of the fluid velocity. Y-component of the fluid velocity. Z-component of the fluid velocity. RHOIC Initial fluid density. PIC TIC 2-62 (CESE) Initial fluid pressure. VARIABLE HIC DESCRIPTION Initial fluid enthalpy. However, when CHEMID refers to a ZND 1- step reaction card, this is the progressive variable (degree of combustion). *CESE_INITIAL_CHEMISTRY_SET Purpose: Initializes the chemistry and fluid state in every element of the specified element set in the CESE mesh that has not already been initialized by *CESE_INITIAL_CHEM- ISTRY_ELEMENT cards. This is only used when chemistry is being solved with the CESE solver. Card 1 1 2 3 4 5 6 7 8 Variable SETID CHEMID COMPID Type I I I Default none none none Card 2 1 Variable UIC 2 VIC 3 4 5 WIC RHOIC PIC 6 TIC 7 HIC 8 Type F F F F F F F Default none none none none none none none VARIABLE DESCRIPTION SETID Identifier of the CESE element set to initialize. CHEMID Identifier of chemistry control card to use. COMPID Identifier of chemical composition to use. UIC VIC WIC X-component of the fluid velocity. Y-component of the fluid velocity. Z-component of the fluid velocity. RHOIC Initial fluid density. PIC TIC 2-64 (CESE) Initial fluid pressure. VARIABLE HIC DESCRIPTION Initial fluid enthalpy. However, when CHEMID refers to a ZND 1- step reaction card, this is the progressive variable (degree of combustion). *CESE_INITIAL_CHEMISTRY_SET Purpose: Define the fluid (gas) properties in a viscous flow for the CESE solver. Material Definition Cards. Include one card for each instance of this material type. This input ends at the next keyword (“*”) card. 4 5 6 7 8 Card 1 1 Variable MID 2 MU Type I F 3 K F Default none none none VARIABLE DESCRIPTION MID MU Material identifier Fluid dynamic viscosity. For Air at 15 °C, MU = 1.81 × 10−5 kg ms⁄ K Thermal conductivity of the fluid Remarks: 1. The viscosity is only used viscous flows, so for inviscid flows, it is not necessary to define it. The thermal conductivity is only used to calculate the heat transfer be- tween the structure and the thermal solver when coupling is activated. 2. As with other solvers in LS-DYNA, the user is responsible for unit consistency. For example, if dimensionless variables are used, MU should be replaced by the corresponding dimensionless one. *CESE Purpose: Define the fluid (gas) properties in a viscous flow for the CESE solver. Include as many cards as needed. This input ends at the next keyword (“*”) card. Card 1 1 Variable MID Type I 2 C1 F 3 C2 F 4 5 6 7 8 PRND F Default none 1.458E- 6 110.4 0.72 VARIABLE DESCRIPTION MID Material identifier C1, C2 Two coefficients in the Sutherland’s formula for viscosity, i.e., 𝜇 = 𝐶1𝑇 𝑇 + 𝐶2 where C1 and C2 are constants for a given gas. For example, for air at moderate temperatures, 𝐶1 = 1.458 × 10−6 kg msK ⁄ 2⁄ , 𝐶2 = 110.4 K PRND The Prandtl Number (used to determine the coefficient of thermal conductivity). It is approximately constant for most gases. For air at standard conditions PRND = 0.72. Remarks: 1. C1 and C2 are only used to calculate the viscosity in viscous flows, so for inviscid flows, this material card is not needed. The Prandtl number is used to extract the thermal conductivity, which is used when thermal coupling with the structure is activated. 2. As with other solvers in LS-DYNA, the user is responsible for unit consistency. For example, if dimensionless variables are used, C1 and C2 should be replaced by the corresponding dimensionless ones. *CESE_MAT_002 Purpose: Define the fluid (gas) properties in a viscous flow for the CESE solver. Material Definition Cards. Include one card for each instance of this material type. This input ends at the next keyword (“*”) card. 6 7 8 Card 1 1 2 3 Variable MID MU0 SMU Type I F F 4 K0 F 5 SK F Default none 1.716E-5 111. 0.0241 194.0 VARIABLE DESCRIPTION MID Material identifier MU0 / SMU Two coefficients appearing in the equation derived by combining Sutherland’s formula with the Power law for dilute gases: 𝜇0 = ( 𝑇0 ) 3 2⁄ 𝑇0 + 𝑆𝜇 𝑇 + 𝑆𝜇 . In the above, MU0 and SMU are parameters characterizing a particular gas. For example, for air at moderate temperatures, 𝜇0 = 1.716 × 10−5 Ns m2⁄ , 𝑆𝜇 = 111 K K0/SK Two coefficients appearing in the equation derived by combining Sutherland’s formula with the Power law for dilute gases: 𝑘0 = ( 𝑇0 ) 3 2⁄ 𝑇0 + 𝑆𝑘 𝑇 + 𝑆𝑘 In the above, K0 and SK are parameters characterizing a particular gas. For example, for air at moderate temperatures, 𝑘0 = 0.0241 W m⁄ , 𝑆𝑘 = 194 K Remarks: 1. The viscosity is only used viscous flows, so for inviscid flows, it is not necessary to define it. The thermal conductivity is only used to calculate the heat transfer be- tween the structure and the thermal solver when coupling is activated. 2. As with other solvers in LS-DYNA, the user is responsible for unit consistency. For example, if dimensionless variables are used, MU should be replaced by the corresponding dimensionless one. *CESE_PART Purpose: Define CESE solver parts, i.e., connect CESE material and EOS information. Part Cards. Include one card for each CESE part. This input ends at the next keyword (“*”) card. Card 1 1 2 3 4 5 6 7 8 Variable PID MID EOSID Type I I I Default none none none VARIABLE DESCRIPTION PID MID Part identifier (must be different from any PID on a *PART card) Material identifier defined by a *CESE_MAT_… card EOSID Equation of state identifier defined by a *CESE_EOS_… card Remarks: 1. Since material coefficients are only used in viscous flows, the MID can be left blank for inviscid flows. *CESE_SURFACE_MECHSSID_D3PLOT Purpose: Identify the surfaces to be used in generating surface D3PLOT output for the CESE solver. These surfaces must be on the outside of volume element parts that are in contact with the CESE fluid mesh. The variables in question are part of the CESE FSI solution process or of the CESE conjugate heat transfer solver. Include as many cards as needed. This input ends at the next keyword (“*”) card. Card 1 1 2 3 4 5 6 7 8 Variable SSID SurfaceLabel Type I Default none VARIABLE SSID A none DESCRIPTION Mechanics solver segment set ID that is in contact with the fluid CESE mesh. SurfaceLabel Name to use in d3plot output to identify the SSID for the LSPP user. *CESE_SURFACE_MECHVARS_D3PLOT Purpose: List of variables to output on the surfaces designated by the segment set IDs given in the *CESE_SURFACE_MECHSSID_D3PLOT cards. Most of the allowed variables are defined only on the fluid-structure interface, and so the segment set IDs defining a portion of the fluid-structure interface must involve only segments (element faces) that are on the outside of volume element parts that are in contact with the CESE fluid mesh. Include as many cards as needed. This input ends at the next keyword (“*”) card. Card 1 1 2 3 4 5 6 7 8 Variable Type Default VARIABLE Output Quantity Output Quantity A none DESCRIPTION Descriptive phrase for the mechanics surface variable to output for the LSPP user. Output will be done on all SSIDs selected by the *CESE_SURFACE_MECHSSID_D3PLOT cards in the problem. Supported variables include: FLUID FSI FORCE FLUID FSI PRESSURE INTERFACE TEMPERATURE SOLID INTERFACE HEAT FLUX FLUID INTERFACE HEAT FLUX INTERFACE HEAT FLUX RATE SOLID INTERFACE DISPLACEMENT SOLID INTERFACE VELOCITY SOLID INTERFACE ACCELERATION Force, displacement, velocity, and acceleration are output as vector quantities. The rest of the variables are scalar quantities. The fluxes are in the normal direction to the fluid/structure interface, with the heat fluxes relative to the normal pointing into the structure. *CHEMISTRY The keyword *CHEMISTRY is used to access chemistry databases that include Chemkin- based descriptions of a chemical model, as well as to select a method of solving the model. The keyword cards in this section are defined in alphabetical order: *CHEMISTRY_COMPOSITION *CHEMISTRY_CONTROL_0D *CHEMISTRY_CONTROL_1D † *CHEMISTRY_CONTROL_CSP *CHEMISTRY_CONTROL_FULL *CHEMISTRY_CONTROL_INFLATOR † *CHEMISTRY_CONTROL_TBX *CHEMISTRY_CONTROL_ZND † *CHEMISTRY_DET_INITIATION † *CHEMISTRY_INFLATOR_PROPERTIES † *CHEMISTRY_MODEL *CHEMISTRY_PATH †: Card may be used only once in a given model An additional option “_TITLE” may be appended to all *CHEMISTRY keywords. If this option is used, then an 80 character string is read as a title from the first card of that keyword's input. At present, LS-DYNA does not make use of the title. Inclusion of titles gives greater clarity to input decks. In order to use one of the chemistry solvers, the input must include at least one *CHEM- ISTRY_MODEL card. For each spatial region containing a different chemical composition, at least one *CHEMISTRY_COMPOSITION card is required. The *CHEMISTRY_CONTROL_0D card is intended to be used in a standalone fashion to verify the validity of a given chemistry model. This model includes the total number of species and all elementary reactions with their Arrhenius rate parameters. For instance, this solver could be used to check the induction time of the model. The *CHEMISTRY_CONTROL_1D, *CHEMISTRY_DET_INITIATION, and *CHEM- ISTRY_CONTROL_ZND cards are intended to provide a one-dimensional initialization to a 2D or 3D chemically-reacting flow. In order to perform a full, general purpose chemistry calculation in 2D or 3D, the *CHEM- ISTRY_CONTROL_FULL card should be used. The *CHEMISTRY_CONTROL_CSP card is an option for reducing the number of species and reactions that are used in a general purpose chemistry calculation. Other reduction mechanisms are planned for the future. An airbag inflator model is available with *CHEMISTRY_CONTROL_INFLATOR along with *CHEMISTRY_INFLATOR_PROPERTIES and a chemistry model that is referenced via three chemical compositions. This involves zero-dimensional modeling, with pyrotechnic inflator, and cold and hot flow hybrid inflator options. The *CHEMISTRY_CONTROL_TBX card is intended for use only in a stochastic particle model, where the *STOCHASTIC_TBX_PARTICLES card is used. *CHEMISTRY Purpose: Provides a general way to specify a chemical composition via a list of species mole numbers in the context of a Chemkin database model. Card 1 Variable 1 ID 2 3 4 5 6 7 8 MODELID Type I I Default none none Species List Card. Provide as many cards as necessary. This input ends at the next keyword (“*”) card. Card 2 1 2 3 4 5 6 7 8 Variable MOLFR Type F Default none SPECIES A none VARIABLE DESCRIPTION ID A unique identifier among all chemistry compositions. MODELID Identifier of a Chemkin-compatible chemistry model. MOLFR SPECIES The number of moles corresponding to the species named in the SPECIES field. But if used with a *STOCHASTIC_TBX_PARTICLES card, it is the molar concentration of the species (in units of moles/[length]3, where “[length]” is the user’s length unit). The Chemkin-compatible name of a chemical species that is defined in the chemistry model identified by MODELID . *CHEMISTRY_CONTROL_0D Purpose: Performs a zero-dimensional isotropic chemistry calculation that operates standalone (does not call the CESE solver). This is for ISOBARIC or ISOCHORIC cases. Card 1 Variable 1 ID 2 3 4 5 6 7 8 COMPID SOLTYP PLOTDT CSP_SEL Type I I I F Default none none none 1.0e-6 Remarks Card 2 Variable 1 DT 2 3 TLIMIT TIC 4 PIC I 0 1 5 RIC 7 8 6 EIC Type F F F F F F Default none none none none none none CSP Parameters Card. Include cards for each chemical species in the following format when CSP_SEL.GT.0. This input ends at the next keyword (“*”) card. Card 3 1 2 3 4 5 6 7 8 Variable AMPL YCUT Type F F Default none none VARIABLE DESCRIPTION ID Identifier for this 0D computation. VARIABLE DESCRIPTION COMPID Chemical composition identifier of composition to use. SOLTYP Type of 0D calculation: EQ.1: Isochoric EQ.2: Isobaric PLOTDT Simulation time interval for output both to the screen and to the isocom.csv file. This file can be loaded into LS-PREPOST for curve plotting using the x-y plot facility. CSP_SEL CSP solver option: EQ.0: Do not use the CSP solver, and ignore the AMPL and YCUT parameters (default). GT.0: Use the CSP solver, with the AMPL and YCUT parameters. DT Initial time step TLIMIT Time limit for the simulation Initial temperature Initial pressure Initial density Initial internal energy Relative accuracy for the mass fraction of a chemical species in the Chemkin input file. Absolute accuracy for the mass fraction of a chemical species in the Chemkin input file. TIC PIC RIC EIC AMPL YCUT Remarks: 1. If CSP_SEL.GT.0, then instead of using the full chemistry solver, the computational singular perturbation (CSP) method solver is used. *CHEMISTRY_CONTROL_1D Purpose: Loads a previously-computed one-dimensional detonation. It is then available for use in the CESE solver for initializing a computation. In the product regions, this card overrides the initialization of the *CESE_INITIAL_CHEMISTRY_… cards. Card 1 Variable 1 ID 2 3 4 5 6 7 8 XYZD DETDIR CSP_SEL Type I F I Default none none none Remarks I 0 1 One-Dimensional Solution LSDA Input File Card. Card 2 1 2 3 4 5 6 7 8 Variable Type FILE A CSP Parameters Card Include cards for each chemical species in the following format when CSP_SEL > 0. This input ends at the next keyword (“*”) card. Card 3 1 2 3 4 5 6 7 8 Variable AMPL YCUT Type F F Default none none VARIABLE DESCRIPTION ID Identifier for this one-dimensional detonation solution. XYZD Position of the detonation front in the DETDIR direction. VARIABLE DESCRIPTION DETDIR Detonation propagation direction EQ.1: 𝑥 EQ.2: 𝑦 EQ.3: 𝑧 CSP_SEL CSP solver option: EQ.0: Do not use the CSP solver, and ignore the AMPL and YCUT parameters (default). GT.0: Use the CSP solver, with the AMPL and YCUT parameters. FILE Name of the LSDA file containing the one-dimensional solution. Relative accuracy for the mass fraction of a chemical species in the chemkin input file. Absolute accuracy for the mass fraction of a chemical species in the chemkin input file. AMPL YCUT Remarks: 1. If CSP_SEL > 0, then instead of using the full chemistry solver, the computational singular perturbation (CSP) method solver is used. *CHEMISTRY_CONTROL_CSP Purpose: Computes reduced chemistry for a specified Chemkin chemistry model using the Computational Singular Perturbation (CSP) method. This card can be used for general- purpose chemical reaction calculations. Card 1 Variable 1 ID 2 3 4 5 6 7 8 IERROPT Type I I Default none none CSP Parameters Card. Include cards for each chemical species in the following format as indicated by the value of IERROPT. This input ends at the next keyword (“*”) card. Card 2 1 2 3 4 5 6 7 8 Variable AMPL YCUT Type F F Default none none VARIABLE DESCRIPTION ID Identifier for this computational singular perturbation solver. IERROPT Selector: EQ.0: AMPL and YCUT values for all chemical species are required. EQ.1: One CSP Parameter Card should be provided, and it will be used for all species. AMPL YCUT Relative accuracy for the mass fraction of a chemical species in the Chemkin input file. Absolute accuracy for the mass fraction of a chemical species in the Chemkin input file. *CHEMISTRY_CONTROL_FULL Purpose: Computes the full chemistry specified by a Chemkin chemistry model. This card can be used for general-purpose chemical reaction calculations. Card 1 Variable 1 ID 2 3 4 5 6 7 8 ERRLIM RHOMIN TMIN Type I F F F Default none none 0.0 0.0 VARIABLE DESCRIPTION ID Identifier for this full chemistry calculation. ERRLIM Error tolerance for the full chemistry calculation. RHOMIN TMIN Minimum fluid density above which chemical reactions are computed. Minimum temperature above which chemical reactions are computed. *CHEMISTRY_CONTROL_INFLATOR Purpose: Provide the required properties of an inflator model for airbag inflation. Card 1 1 2 3 4 5 6 7 8 Variable MODEL OUT_TYPE TRUNTIM DELT PTIME Type Remarks I 1 I F F F 2,4 Inflator Output Database File (an ASCII file) Card. Card 2 1 2 3 4 5 6 7 8 Variable Type FILE A Densities for Condensed Species. Include as many cards as needed. This input ends at the next keyword (“*”) card. Card 3 1 2 3 4 5 6 7 8 Variable DENSITY Species Name Type F Default none Remark VARIABLE 3-10 (CHEMISTRY) A none VARIABLE DESCRIPTION MODEL Type of inflator model to compute. EQ.1: EQ.2: Pyrotechnic model Hybrid model with cold flow option in the gas chamber EQ.3: Hybrid model with heat flow in the gas chamber OUT_TYPE Selects the output file format that will be used in an airbag simulation. EQ.0: EQ.1: EQ.2: EQ.3: EQ.4: Screen output CESE compressible flow solver (default) ALE solver CPM solver (with 2nd-order expansion of C p ) CPM solver (with 4th-order expansion of C p ) TRUNTIM Total run time. DELT Delta(t) to use in the model calculation. PTIME Time interval for output of time history data to FILE. FILE Name of the ASCII file in which to write the time history data and other data output by the inflator simulation. DENSITY Density of a condensed-phase species present in the inflator. Chemkin-compatible name of a condensed-phase species. Species Name Remarks: 1. If MODEL = 3, the solution of an elementary reaction system is required for the finite-rate chemistry in the gas chamber. 2. Output file includes all of the necessary thermodynamics variables and load curves for the species mass flow rate, temperature, and density curve. This will make it possible to generate the velocity curve which is required by each solver that carries out an airbag simulation. 3. At least one of these cards will be input if condensed-phase species are present during the propellant combustion. In this case, the user must specify each con- densed-phase density. This density is then used to compute the volume fractions in both the combustion and gas chamber, where the energy equations are needed. 4. If OUT_TYPE = 0, the propellant information will be displayed on the screen, including total mass, remaining mass percentage, and mass burning rate versus time. With this option, the user can quickly see the effect of changing the parame- ters on the first three *CHEMISTRY_INFLATOR_PROPERTIES cards. *CHEMISTRY Purpose: Specify a chemistry solver for use in conjunction with stochastic TBX particles. This is intended only for modeling the second phase of an explosion where the explosive has embedded metal (aluminum) particles that are too large to have burned in the first phase of the explosion. This chemistry card points to a *CHEMISTRY_MODEL card (via IDCHEM) with its associated *CHEMISTRY_COMPOSITION cards to set up the initial conditions. That is, it establishes the spatial distribution of the species in the model. It is assumed that there is no chemical reaction rate information in the chemistry model files. This is done since a special chemical reaction mechanism is implemented for TBX modeling. If particles other than solid aluminum particles are embedded in the explosive, then another burn model has to be implemented. Surface Part Card. Card 1 format used when the PART keyword option is active. Card 1 1 2 3 4 5 6 7 8 Variable IDCHEM USEPAR Type I Default none I 1 VARIABLE DESCRIPTION IDCHEM Identifier for this chemistry solver. USEPAR Coupling flag indicating if a *STOCHASTIC_TBX_PARTICLES card is provided for this model: EQ.1: uses a *STOCHASTIC_TBX_PARTICLES card (default). EQ.0: does not use such a card. *CHEMISTRY_CONTROL_ZND Purpose: Computes the one-dimensional reduced chemistry of a ZND model. It is then used in the initialization of the chemistry part of the CESE solver. When this card is used, the *CESE_INITIAL_CHEMISTRY… cards must specify the progressive variable (degree of combustion) in the HIC field. Card 1 Variable 1 ID Type I Default none Card 2 Variable Type 1 F F 2 3 4 5 6 7 8 2 EPLUS 3 Q0 4 5 6 7 8 GAM XYZD DETDIR F F F F I Default none none none none none none VARIABLE DESCRIPTION ID F Identifier for this full chemistry calculation. Overdriven factor EPLUS EPLUS parameter of the ZND model. Q0 Q0 parameter of the ZND model. GAM XYZD GAM parameter of the ZND model. Position of the detonation front in the DETDIR direction. DETDIR Detonation propagation direction (1 => X; 2 => Y; 3 => Z) *CHEMISTRY_DET_INITIATION Purpose: Performs a one-dimensional detonation calculation based upon a chemical composition and initial conditions. It is then available for use immediately in the CESE solver for initializing a computation, or it can be subsequently used by the *CHEMISTRY_- CONTROL_1D card in a later run. In the product regions, this card overrides the initialization of the *CESE_INITIAL_CHEMISTRY… cards. Card 1 Variable 1 ID 2 3 4 5 6 7 8 COMPID NMESH DLEN CFL TLIMIT XYZD DETDIR Type I I I F F F F I Default none none none none none none none none LSDA Output File Card. Card 2 1 2 3 4 5 6 7 8 Variable Type FILE A VARIABLE DESCRIPTION ID Identifier for this one-dimensional detonation computation. COMPID Chemical composition identifier of composition to use. NMESH Number of equal-width elements in the one-dimensional domain. DLEN Length of the one-dimensional domain. CFL Time-step limiting factor. TLIMIT Time limit for the simulation XYZD Position of the detonation front in the DETDIR direction. DETDIR Detonation propagation direction (1 => X; 2 => Y; 3 => Z) VARIABLE FILE DESCRIPTION Name of the LSDA file in which to write the one-dimensional solution. *CHEMISTRY_INFLATOR_PROPERTIES Purpose: Provide the required properties of an inflator model. Card 1 1 2 3 4 5 6 7 8 Variable COMP_ID PDIA PHEIGHT PMASS TOTMASS Type Remarks I 1 F F F F Card 2 1 2 3 4 5 6 7 8 Variable TFLAME PINDEX A0 TDELAY RISETIME Type F F F F F Default none none none none None Combustion Chamber Parameter Card. Card 3 1 2 3 4 Variable COMP1ID VOL1 AREA1 CD1 Type I F F F 5 P1 F 6 7 8 T1 DELP1 F F Default none none none none none none none Gas Plenum Parameter Card. Card 4 1 2 3 4 Variable COMP2ID VOL2 AREA2 CD2 Type I F F F 5 P2 F 6 7 8 T2 DELP2 F F Default none none none none none none none Tank Parameter Card. Card 5 1 2 3 Variable COMP3ID VOL3 P3 Type I F F 4 T3 F Default none none none none 5 6 7 8 VARIABLE COMP_ID DESCRIPTION Chemical composition identifier of the composition for the steady- state propellant combustion . PDIA Propellant diameter. PHEIGHT Propellant height. PMASS Individual cylinder propellant mass. TOTMASS Total propellant mass. TFLAME Adiabatic flame temperature. PINDEX Power of the pressure in rate of burn model. A0 Steady-state constant. TDELAY Ignition time delay. VARIABLE DESCRIPTION RISETIME Rise time. COMP1ID Chemical composition identifier of composition to use in the combustion chamber. VOL1 Volume of the combustion chamber. AREA1 Area of the combustion chamber. CD1 Discharge coefficient of the combustion chamber. P1 T1 Pressure in the combustion chamber. Temperature in the combustion chamber. DELP1 Rupture pressure in the combustion chamber. COMP2ID Chemical composition identifier of composition to use in the gas plenum. VOL2 Volume of the gas plenum. AREA2 Area of the gas plenum. CD2 Discharge coefficient of the gas plenum. P2 T2 Pressure in the gas plenum. Temperature in the gas plenum. DELP2 Rupture pressure in the gas plenum. COMP3ID Chemical composition identifier of composition to use in the tank. VOL3 Volume of the tank. P3 T3 Pressure in the tank. Temperature in the tank. Remarks: 1. The propellant composition can be obtained by running a chemical equilibrium program such as NASA CEA, the CHEETAH code, or the PEP code. LSTC pro- vides a modified version of the PEP code along with documentation for users; it is available upon request. *CHEMISTRY Purpose: Identifies the files that define a Chemkin chemistry model. Card 1 1 2 3 4 5 6 7 8 Variable MODELID JACSEL ERRLIM Type I Default none I 1 F 1.0e-3 Chemkin Input File Card. Card 2 1 2 3 4 5 6 7 8 Variable Type FILE1 A Thermodynamics Database File Card. Card 3 1 2 3 4 5 6 7 8 Variable Type FILE2 A Transport Properties Database File Card. Card 4 1 2 3 4 5 6 7 8 Variable Type FILE3 A VARIABLE DESCRIPTION MODELID Identifier for this Chemkin-based chemistry model.. VARIABLE DESCRIPTION JACSEL Selects the form of the Jacobian matrix for use in the source term. EQ.1: Fully implicit (default) EQ.2: Simplified implicit ERRLIM Allowed error in element balance in a chemical reaction. FILE1 FILE2 FILE3 Name of the file containing the Chemkin-compatible input. Name of the file containing the chemistry thermodynamics database. Name of the file containing the chemistry transport properties database. *CHEMISTRY Purpose: To specify one or more search paths to look for chemistry database files. Include as many cards as needed. This input ends at the next keyword (“*”) card. Card 1 1 2 3 4 5 6 7 8 Variable Type DIR A VARIABLE DESCRIPTION DIR Directory path to add to the search set. *EM The *EM keyword cards provide input for a new electromagnetism module for solving 3D eddy-current, inductive heating or resistive heating problems, coupled with mechanical and thermal solvers. Typical applications include magnetic metal forming and welding. A boundary element method in the air is coupled to finite elements in the conductor in order to avoid meshing the air. *EM_2DAXI *EM_BOUNDARY *EM_CIRCUIT *EM_CIRCUIT_CONNECT *EM_CIRCUIT_RANDLE *EM_CIRCUIT_ROGO *EM_CONTACT *EM_CONTACT_RESISTANCE *EM_CONTROL *EM_CONTROL_CONTACT *EM_CONTROL_SWITCH *EM_CONTROL_SWITCH_CONTACT *EM_CONTROL_TIMESTEP *EM_DATABASE_CIRCUIT *EM_DATABASE_CIRCUIT0D *EM_DATABASE_ELOUT *EM_DATABASE_FIELDLINE *EM_DATABASE_GLOBALENERGY *EM_DATABASE_NODOUT *EM_DATABASE_PARTDATA *EM_DATABASE_POINTOUT *EM_DATABASE_ROGO *EM_DATABASE_TIMESTEP *EM_EOS_BURGESS *EM_EOS_MEADON *EM_EOS_PERMEABILITY *EM_EOS_TABULATED1 *EM_EOS_TABULATED2 *EM_EXTERNAL_FIELD *EM_ISOPOTENTIAL *EM_ISOPOTENTIAL_CONNECT *EM_MAT_001 *EM_MAT_002 *EM_MAT_003 *EM_MAT_004 *EM_OUTPUT *EM_POINT_SET *EM_RANDLE_SHORT *EM_ROTATION_AXIS *EM_SOLVER_BEM *EM_SOLVER_BEMMAT *EM_SOLVER_FEM *EM_SOLVER_FEMBEM *EM_VOLTAGE_DROP *EM Purpose: Sets up the electromagnetism solver as 2D axisymmetric instead of 3D, on a given part, in order to save computational time as well as memory. The electromagnetism is solved in 2D on a given cross section of the part (defined by a segment set), with a symmetry axis defined by its direction (at this time, it can be the 𝑥, 𝑦, or 𝑧 axis). The EM forces and Joule heating are then computed over the full 3D part by rotations. The part needs to be compatible with the symmetry, i.e. each node in the part needs to be the child of a parent node on the segment set, by a rotation around the axis. Only the conductor parts (with a *EM_MAT_… of type 2 or 4) should be defined as 2D axisymmetric. Card 1 1 2 3 4 5 6 7 8 Variable PID SSID STARSSID ENDSSID NUMSEC Type I I I I I Default none none none none none VARIABLE DESCRIPTION Part ID of the part to be solved using 2D axisymmetry Segment Set ID : Segment that will define the 2D cross section of the part where the EM field is solved Used by the 2D axisymmetric solver to make the connection between two corresponding boundaries on each side of a slice when the model is a slice of the full 360 circle. Number of Sectors. This field gives the ratio of the full circle to the angular extension of the mesh. This has to be a power of two. For example, NUMSEC = 4 means that the mesh of the part represents one fourth of the total circle. If this value is set to 0, then the value from *EM_ROTATION_AXIS is used instead. PID SSID STARSSID, ENDSSID NUMSEC Remarks: 1. At this time, either all or none of the conductor parts should be 2D axisymmetric. In the future, a mix between 2D axisymmetric and 3D parts will be allowed. *EM_BOUNDARY Purpose: Define some boundary conditions for the electromagnetism problems. Include as many cards as needed. This input ends at the next keyword (“*”) card. Card 1 1 2 3 4 5 6 7 8 Variable SSID BTYPE Type I I Default none none VARIABLE DESCRIPTION SSID Segment Set Id BTYPE EQ.9: The faces of this segment set are eliminated from the BEM calculations (used for example for the rear or side faces of a workpiece). Available options include SOURCE Purpose: Define an electrical circuit. *EM For the SOURCE option, the current will be considered uniform in the circuit. This can be useful in order to save computational time in cases with a low frequency current and where the diffusion of the EM fields is a very fast process. This option is in contrast with the general case where the current density in a circuit is completed in accordance with the solver type defined in EMSOL of *EM_CONTROL. For example, if an eddy current solver is selected, the diffusion of the current in the circuit is taken into account. Card 1 1 2 3 Variable CIRCID CIRCTYP LCID 4 R/F 5 L/A 6 C/to Type I I I F F F 7 V0 F 8 T0 F Default none none none none none none none 0. Card 2 1 2 3 4 5 6 7 8 Variable SIDCURR SIDVIN SIDVOUT PARTID Type I I I I Default none none none none VARIABLE DESCRIPTION CIRCID Circuit ID VARIABLE DESCRIPTION CIRCTYP Circuit type: EQ.1: Imposed current vs time defined by a load curve. EQ.2: Imposed voltage vs time defined by a load curve. EQ.3: R, L, C, V0 circuit. EQ.11: Imposed current defined by an amplitude A, frequency F and initial time 𝑡0: 𝐼 = 𝐴sin[2𝜋𝐹(𝑡 − 𝑡0)] EQ.12: Imposed voltage defined by an amplitude A, frequency F and initial time 𝑡0: 𝑉 = 𝐴sin[2𝜋𝐹(𝑡 − 𝑡0)] EQ.21: Imposed current defined by a load curve over one period and a frequency F EQ.22: Imposed voltage defined by a load curve over one period and a frequency F Load curve ID for CIRCTYP = 1, 2, 21 or 22 Value of the circuit resistance for CIRCTYP = 3 Value of the Frequency for CIRCTYP = 11, 12, 21 or 22 Value of the circuit inductance for CIRCTYP = 3 Value of the Amplitude for CIRCTYP = 11 or 12. To have the amplitude defined by a load curve, a negative value can be entered and the solver will look for the corresponding Load Curve ID. Value of the circuit capacity for CIRCTYP = 3 Value of the initial time t0 for CIRCTYP = 11 or 12 Value of the circuit initial voltage for CIRCTYP = 3. Starting time for CIRCTYPE = 3. Default is at the beginning of the run. Segment set ID for the current. It uses the orientation given by the normal of the segments. To use the opposite orientation, use a '–' (minus) sign in front of the segment set id. CIRCTYP.EQ.1/11/21: The current is imposed through this CIRCTYP.EQ.3: segment set the circuit The current needed by equations is measured through this seg- ment set. LCID R/F L/A C/t0 V0 T0 SIDCURR SIDVIN *EM DESCRIPTION Segment set ID for input voltage or input current when CIRCTYP.EQ.2/3/12/22 and CIRCTYP.EQ 1/11/21 respectively. It is considered to be oriented as going into the structural mesh, irrespective of the orientation of the segment. SIDVOUT Segment set ID for output voltage or output current when CIRCTYP = 2/3/12/22 and CIRCTYP = 1/11/21 respectively. It is considered to be oriented as going out of the structural mesh, irrespective of the orientation of the segment. PARTID Part ID associated to the Circuit. It can be any part ID associated to the circuit. Circuit Type (CIRCTYP) Variable 1: Current Imposed Imposed 2: Voltage 3: R, L, C 11: F, A, t0 12: F, A, t0 LCID R/L/C/V0 F A/t0 SIDCURR SIDVIN SIDVOUT PARTID M - - - M M* M* M M - - - O M M M Variable 21: LCID, F 22 : LCID, F LCID R/L/C/V0 F A/t0 SIDCURR SIDVIN SIDVOUT PARTID M - M - M M* M* M M - M - O M M M - M - - M M M M - - - - - - - - - - M M M M* M* M - - - - - - - - - - M M O M M M - - - - - - - - Table 4-1. Correspondence between circuit type and card entries. “M” indicates mandatory, “M*” mandatory with exceptions , “O” indicates optional, and “-” indicates ignored. Remarks: 1. When defining a circuit with an imposed current (type 1, 11 or 21) in cases of a closed loop geometry (torus), SIDVIN and SIDVOUT cannot be defined and thus, only SIDCURR is necessary. 2. When defining a circuit with an imposed tension (type 2, 12, 22), it is possible to also define SIDCURR. This can be useful in circuits where various flow paths are possible for the current in order to force the entire current to go through SIDCURR. 3. Circuit types 21 and 22 are for cases where the periodic current/tension does not exactly follow a perfect sinusoidal. The user has to provide the shape of the cur- rent/tension over one period through a LCID as well as the frequency. *EM_CIRCUIT Purpose: This keyword connects several circuits together by imposing a linear constraint on the global currents of circuit pairs This is especially useful for 2D axisymmetric models involving spiral or helical coils. 𝑐1𝑖1 + 𝑐2𝑖2 = 0. Card 1 1 2 3 4 Variable CONID CONTYPE CIRC1 CIRC2 Type I I I I 5 C1 F 6 C2 F 7 8 Default none none none none none none VARIABLE DESCRIPTION CONID Id of the Circuit Connect CONTYPE Type of connection between circuits. For the moment, it is only possible to combine circuits by imposing a linear constraint on the global current (=1). C1/C2 Values of the linear constraints if CONTYPE = 1. *EM Purpose: define the distributed Randle circuit parameters for a unit Randle cell. Card 1 1 2 3 4 5 6 7 8 Variable RDLID RDLTYPE RDLAREA ISSID1 ISSID2 SEPPART ANOPART CATPART Type I I I I I I I I Default none none none none none none none none Card 2 Variable Type 1 Q F 2 3 4 5 6 7 8 CQ SOCINIT SOCTOU F F F Default none none none none Card 3 1 2 3 4 5 6 7 8 Variable R0CHA R0DIS R10CHA R10DIS C10CHA C10DIS Type F F F F F F Default none none none none none none Card 4 1 2 3 4 5 6 7 8 Variable TEMP FRTHERM R0TOTH DUDT TEMPU Type F I I F I Default none none none none none Card 5 1 2 3 4 5 6 7 8 Variable USESOCS TAUSOCS SICSLCID Type I F I Default none none none VARIABLE DESCRIPTION RDLID Id of the Randle Cell RDLTYPE Type of Randle Cell RDLAREA Randle Area: EQ.0: Default.The parameters are not scaled by area factors. EQ.1: The parameters are per unit area and will be scaled in each Randle circuit by a factor depending on the local area of the circuit. EQ.2: The parameters are defined for the whole unit cell and will be scaled in each Randle circuit by a factor depending on the local area of the circuit and the global area of the cell. ISSID1 ISSID2 Segment set ID defining the anode side on the current collector. Segment set ID defining the cathode side on the current collector. SEPPART Separator Part ID ANOPART Anode Part ID CATPART Cathode Part ID Q CQ Unit cell capacity. SOC conversion factor (%/s), known to be equal to 1/36 in S.I units. SOCINIT Initial state of charge of the unit cell. VARIABLE SOCTOU DESCRIPTION Constant value if positive or load curve ID if negative integer defining the equilibrium voltage (OCV) as a function of the state of charge (SOC). R0CHA/ R10CHA/ C10CHA Constant if positive value or load curve or table id (if negative integer) defining r0/r10/c10 when the current flows in the charge direction as a function of: -SOC if load curve -SOC and Temperature if table. R0DIS/ R10DIS/ C10DIS Constant if positive value or load curve or table id (if negative integer) defining r0/r10/c10 when the current flows in the discharge direction as a function of: -SOC if load curve -SOC and Temperature if table. TEMP Constant temperature value used for the Randle circuit parameters in case there is no coupling with the thermal solver (FRTHERM = 0) FRTHERM From Thermal : EQ.0: The temperature used in the Randle circuit parameters is TEMP EQ.1: The temperature used in the Randle circuit parameter is the temperature from the thermal solver. R0TOTH R0 to Thermal : EQ.0: The joule heating in the resistance r0 is not added to the thermal solver EQ.1: The joule heating in the resistance r0 is added to the thermal solver DUDT If negative integer, load curve ID of the reversible heat as a function of SOC. TEMPU Temperature Unit : EQ.0: The temperature is in Celsius EQ.1: The Temperature is in Kelvin VARIABLE DESCRIPTION USESOCS Use SOC shift : EQ.0: Don't use the added SOCshift EQ.1: Use the added SOCshift TAUSOCS Damping time in the SOCshift equation SOCSLCID Load curve giving f(i) where I is the total current in the unit cell Remarks: 1. Sometimes, an extra term called SOCshift (or SocS) can be added at high rate discharges to account for diffusion limitations. The SOCshift is added to SOC for the calculation of the OCV u(SOC+SOCshift) and r0(Soc+SOCshift). SOCshift satisfies the following equation: d(SOCshift)/dt + SOCshift/tau = f(i(t))/tau with SOCshift(t = 0)=0 *EM Purpose: Define Rogowsky coils to measure a global current vs time through a segment set or a node set. Include as many cards as needed. This input ends at the next keyword (“*”) card. Card 1 1 2 3 4 5 6 7 8 Variable ROGID SETID SETTYPE CURTYP Type Default I 0 I 0 I 0 I 0 VARIABLE DESCRIPTION ROGID Rogowsky coil ID SETID Segment or node set ID SETTYPE Type of set: EQ.1: Segment set EQ.2: Node set (not available yet} CURTYP Type of current measured: EQ.1: Volume current EQ.2: Surface current (not available yet} EQ.3: Magnetic field flow (B field times Area) Remarks: 1. An ASCII file “em_rogo_xxx” , with xxx representing the rogoId, is generated for each *EM_CIRCUIT_ROGO card giving the value of the current or the magnetic field vs time. *EM_CONTACT Purpose: Optional card used for defining and specifying options on electromagnetic contacts between two sets of parts. Generally used with the *EM_CONTACT_RESIS- TANCE card. Fields left empty on this card default to the value of the equivalent field for the *EM_CONTROL_CONTACT keyword. Contact Definition Cards. Include one card for each contact definition. This input ends at the next keyword (“*”) card. Card 1 1 2 3 4 5 6 7 Variable CONTID COTYPE PSIDM PSIDS EPS1 EPS2 EPS3 8 D0 Type I Default none I 0 I I F F F F none none 0.3 0.3 0.3 None VARIABLE DESCRIPTION CONTID Electromagnetic contact ID COTYPE Type of EM contact EQ.0: Contact type 0 (Default). EQ.1: Contact type 1. PSIDM Master part set ID PSIDS EPSi Slave part set ID Contact Coefficients for contact detection conditions. See discussion below. D0 Contact condition 3 when COTYPE = 1. Remarks: Contact is detected when all of the following three condition are satisfied: 1. Contact condition 1: 𝒏1. 𝒏2 ≤ −1 + 𝜀1 Figure 4-2. Contact detection conditions between two faces. 2. Contact condition 2: −𝜺2 ≤ 𝛼1 ≤ 1 + 𝜀2 −𝜺2 ≤ 𝛼2 ≤ 1 + 𝜀2 −𝜺2 ≤ 𝛼3 ≤ 1 + 𝜀2 With 𝑛1 and 𝑛2 the normal vectors of faces 𝑓1 and 𝑓2 respectfully and 𝑃 the projec- tion of point 𝑎2 on face 𝑓1 with (𝛼1, 𝛼2, 𝛼3) its local coordinates . 3. Contact condition 3 depends on the contact type. a) For contact type 0: 𝑑 ≤ 𝜀3𝑆1 where 𝑑 is the distance between 𝑃 and 𝑎2 and where 𝑆1 the minimum side length: 𝑆1 = min[𝑑(𝑎1, 𝑏1), 𝑑(𝑏1, 𝑐1), 𝑑(𝑐1, 𝑎1)] b) For contact type 1 : 𝑑 ≤ 𝐷0 *EM_CONTACT_RESISTANCE Purpose: Calculate the contact resistance of a previously defined EM contact in *EM_CON- TACT. Most contact resistance calculations are based on Ragmar Holm’s “Electric Contacts”. Card 1 1 2 3 4 5 6 7 8 Variable CRID CONTID CTYPE CIRCID JHRTYPE Type I I I I I Default none none none none none Card 2 if CTYPE = 1. Cards 2 1 2 3 4 5 6 7 8 Variable LCID Type I Default none Card 2 if CTYPE = 2. Cards 2 1 2 3 4 5 6 7 8 Variable RHO RAD Type F Default 0. F 0. Cards 2 1 2 Variable RHO RAD Type F Default 0. F 0. Card 2 if CTYPE = 4. Cards 2 1 2 Variable RHO RAD Type F Default 0. F 0. Card 2 if CTYPE = 5. 3 D F 0. 3 D F 0. 4 5 CURLCID EPS I 0 4 CURLCID I 0 F 0. 5 E F 0. *EM 7 8 6 HB F 0. 6 7 8 CURV F 0. Cards 2 1 2 3 4 5 6 7 8 Variable RHOPROB RHOSUB RHOOXY FACTE FACFILM Type F F F F F Default none none none none none VARIABLE DESCRIPTION CRID Resistive contact ID CONTID EM contact ID defined in *EM_CONTACT VARIABLE DESCRIPTION CTYPE Contact Resistance type : EQ.1: Contact resistance defined by user defined load curve. EQ.2: Classic Holm’s formula for contact resistances . EQ.3: Modified contact resistance for cases with plastic deformation in the contact area . EQ.4: Modified contact resistance for cases with elastic deformation in the contact area . EQ.5: Basic contact resistance definition . CIRCID Circuit ID: When defined, the contact resistance will be added to the corresponding circuit total resistance and taken into account in the circuit equations. JHRTYPE Indicates how the Joule heating calculated by the contact resistance shall be taken into account: EQ.0: No addition: The Joule heating calculated by the contact resistance is not taken into account. EQ.1: The Joule heating coming from the contact resistance is divided and distributed evenly among all elements neigh- boring the contact surface. Load Curve ID defining the contact resistance versus time. Material resistivity ρmat. If not defined or EQ. 0.0, the solver will automatically calculate an average resistivity based on the conductivity of the elements that are in contact. Radius of the contact sphere a. If not defined or EQ. 0.0, the solver will automatically calculate an equivalent radius based on the contact area: 𝑎 = √Area 𝜋⁄ . LCID RHO RAD D Diameter of the Electrode. CURLCID Load Curve ID defining the current intensity of the electrode. If not defined or EQ. 0, the solver will automatically look for the circuit’s current intensity using the circuit defined in CIRID. EPS HB 4-20 (EM) Constant 𝜀 with values typically between 0.35 and 1. VARIABLE DESCRIPTION E Material Young’s modulus. CURV Radius of curvature of the contact surface, 𝑟. RHOPROB Probe resistivity, 𝜌prob RHOSUB Substrate resistivity, 𝜌sub RHOOXY Film resistivity, 𝜌oxi Scale factor on the constriction area when calculating the constriction resistance. If negative, the factor is time-dependent and defined by the load curve absolute value (FACTE). Scale factor on the constriction area when calculating the film resistance. If negative, the factor is time-dependent and defined by the load curve absolute value (FACFILM). FACTE FACFILM Remarks: 1. Holm’s formula for Contact Resistance. A very good approximation of the electric contact resistance is given by Holm’s formula : 𝑅contact = ρmat 2a where ρmat is the material’s resistivity and a is the radius of the contact surface assuming the contact surface area is close to that of a circle : Area = 𝜋𝑎2. It is recommended to use this method (CTYPE = 2) in a first approach since most other contact resistance definitions are extensions of this formula. 2. Contact Area formulations. For certain types of applications such as resistance spot welding (RSW) it is advantageous to better approximate the area by taking into account the deformation and the heterogeneities of the materials that come into contact at a microscopic level. For a plastic deformation of the contact zone, the contact area, assumed to be circular, can be defined approximated as: Area = 𝐹𝑐 𝜀 𝐻𝑏 where 𝐹𝑐 is the contact force, 𝜀 a constant with values between 0.35 and 1, and 𝐻𝑏 the Brinell hardness of the material. For an elastic deformation in the contact area, the radius of the contact surface is now given by: 2a Current flow Electrode Lorentz Force: Fc Curvature of the current lines induces a Lorentz Force Contact Area Workpiece Figure 4-3. Electrode coming into contact with workpiece (RSW application). 𝑎 = 1/3 𝑟𝐹𝑐 where 𝑟 is the radius of curvature of the contact surface and E is Young’s modulus. The Holm formula can then be modified in order to give: and 𝑅contact = ρmat × √ 𝜋𝜀𝐻𝑏 𝐹𝑐 𝑅contact = ρmat × ( 𝑟𝐹𝑐 1/3 ) in the cases of plastic (CTYPE = 3) and elastic (CTYPE = 4) deformations respect- fully. 3. Lorentz Force from a Spherical Electrode. When a spherical electrode comes into contact with a work piece, the curvature of the current flowing from the elec- trode to the work piece induces a Lorentz force parallel to the normal of the con- tact surface thus forcing the electrode and the work piece away from each other. Its intensity can be written as: 𝐹𝑐 = 𝜇0 4𝜋 𝐼2 ln ( 2𝑎 ) where 𝐼 is the current intensity and 𝐷 the diameter of the electrode. See Figure 4-3. 4. Basic resistive contact formulation (CTYPE = 5). In the case of a clean metal contact with no film the resistance calculation involves only the constriction term. If a film is present and both sides have different metals, the contact resistance, 𝑅contact, is the sum of the constriction resistance 𝑅constriction and the film resistance 𝑅film. In the basic resistive model, the following expressions determine the re- sistance: 𝑅constriction = ρprob+ρsub √FACTE × ContactArea 𝑅film = 𝜌oxy √FACFILM × ContactArea 𝑅contact = 𝑅constriction + 𝑅film. Purpose: Enable the EM solver and set its options. *EM_CONTROL Card 1 1 2 3 4 5 6 7 8 Variable EMSOL NUMLS MACRODT Type Default I 0 I F 100 none VARIABLE DESCRIPTION EMSOL Electromagnetism solver selector: EQ.1: Eddy current solver EQ.2: Induced heating solver EQ.3: Resistive heating solver NUMLS Number of local EM steps in a whole period for EMSOL = 2. Not used for EMSOL = 1 MACRODT Macro time step when EMSOL = 2. Can be used as constant EM time step when EMSOL = 1. Obsolete: use *EM_CONTROL_- TIMESTEP. *EM Purpose: This keyword activates the electromagnetism contact algorithms, which detects contact between conductors. Electromagnetic fields to flow from one conductor to another when detected as in contact. Card 1 1 2 3 4 5 6 7 Variable EMCT CCONLY COTYPE EPS1 EPS2 EPS3 8 D0 Type Default I 0 I 0 I 0 F F F F 0.3 0.3 0.3 none VARIABLE DESCRIPTION EMCT EM contact activation flag: EQ.0: No contact detection EQ.1: Contact detection CCONLY Determines on which parts of the model the EM contact should be activated. EQ.0: Contact detection between all active parts associated with a conducting material. (Default) EQ.1: Only look for EM contact between parts associated through the EM_CONTACT card. In some cases this option can reduce the calculation time. COTYPE Type of EM contact. If *EM_CONTACT is not defined, the solver will look for global contact options in *EM_CONTROL_CONTACT. EQ.0: Contact type 0 (Default). EQ.1: Contact type 1. EPSi Global contact coefficients used if the equivalent fields in *EM_- CONTACT are empty. D0 Global contact condition 3 value when COTYPE = 1 *EM_CONTROL_SWITCH Purpose: It is possible to active a control “switch” that will shut down the solver based on a load curve information. LS-DYNA incorporates complex types of curves that allow the setting up of complex On/Off switches, for instance, by using a nodal temperature value. Card 1 1 2 3 4 5 6 7 8 Variable LCID FEMCOMP BEMCOMP Type Default I 0 I 0 I 0 VARIABLE DESCRIPTION LCID Load Curve ID. Negative values switch the solver off, positive values switch it back on. FEMCOMP Determines if FEM matrices are recomputed each time the EM solver is turned back on : EQ.0 : FEM matrices are recomputed EQ.1 : FEM matrices are not recomputed BEMCOMP Determines if BEM matrices are recomputed each time the EM solver is turned back on : EQ.0 : BEM matrices are recomputed EQ.1 : BEM matrices are not recomputed *EM Purpose: It is possible to active a control “switch” that will shut down the electromagnetic contact detection. This can be useful in order to save some calculation time in cases where the user knows when contact between conductors will occur or stop occurring. Card 1 1 2 3 4 5 6 7 8 Variable LCID NCYLFEM NCYLFEM Type Default I 0 I 0 I 0 VARIABLE DESCRIPTION LCID Load Curve ID. Negative values switch the contact detection off, positive values switch it back on. NCYLFEM NCYLBEM Determines the number of cycles before FEM matrix recomputation. If defined this will overwrite the previous NCYCLFEM as long as the contact detection is turned on. Determines the number of cycles before BEM matrix recomputa- tion. If defined this will overwrite the previous NCYCLBEM as long as the contact detection is turned on. Purpose: Controls the EM time step and its evolution *EM_CONTROL_TIMESTEP Card 1 1 2 3 4 5 6 7 8 Variable TSTYPE DTCONS LCID FACTOR Type I F I F Default none none none 1.0 VARIABLE DESCRIPTION TSTYPE Time Step type EQ.1: constant time step given in DTCONST EQ.2: time step vs time given by a load curve specified in LCID EQ.3: automatic time step computation, depending on the solver type. This time step is then multiplied by FACTOR DTCONST Constant value for the time step for TSTYPE = 1 LCID Load curve ID giving the time step vs time for TSTYPE = 2 FACTOR Multiplicative factor applied to the time step for TSTYPE = 3 Remarks: 1. For an eddy current solver, the time step is based on the diffusion equation for the magnetic field. ∂𝐴⃗ ∂𝑡 + ∇⃗⃗⃗⃗⃗ × ∇⃗⃗⃗⃗⃗ × 𝐴⃗ + 𝜎∇⃗⃗⃗⃗⃗𝜑 = 𝚥 ⃗𝑆 It is computed as the minimal elemental diffusion time step over the elements. For a given element, the elemental diffusion time step is given as 𝑑𝑡𝑒 = 𝑙𝑒 ⁄ , where: 2𝐷 • D is the diffusion coefficient 𝐷 = 1 ⁄ 𝜇0𝜎𝑒 , • 𝜎𝑒 is the element electrical conductivity, • 𝜇0 is the permeability of free space, • 𝑙𝑒 is the minimal edge length of the element (minimal size of the element). *EM_DATABASE_CIRCUIT Purpose: This keyword enables the output of EM data for every circuit defined. Output options card Card 1 1 2 3 4 5 6 7 8 Variable OUTLV DTOUT Type Default I 1 F 0. VARIABLE DESCRIPTION OUTLV Determines if the output file should be dumped. EQ.0: No output file is generated. EQ.1: The output file is generated. DTOUT Time interval to print the output. If DTOUT is equal to 0.0, then the EM timestep will be used. Remarks: 1. The file name for this database is em_circuit_XXX.dat with XXX the circuit ID. 2. ResistanceD is calculated in the following way: a) A scalar potential difference of 1 is imposed at the circuit’s boundaries SIDVIN and SIDVOUT. b) The system to be solved at SIDCURR is then ∇2𝜑 = 0 with 𝜑SIDVIN = 1 and 𝜑SIDVOUT = 0. No diffusive effects are taken into account meaning that the current density can be written as 𝐣 = ∇𝜑 and the total current as 𝐼 = 𝐣 ⋅ 𝐧𝑑𝐴. c) The resistance can then be estimated using 𝑅𝐷 = 𝑈 𝐼⁄ . The calculation of this 𝑅𝐷 resistance is solely based on the circuit’s geometry and conductivi- ty. It is therefore equivalent to the resistance as commonly defined in the circuit equations: 𝑅𝐷 = 𝐿 𝜎𝑆⁄ where L is the length of the circuit and S its surface area. 3. ResistanceJ is calculated by using the data provided during the EM solve : 𝑅𝐽 = 𝐽 𝐼2⁄ where J and I are, respectively, the joule heating and the current. Com- pared with ResistanceD, ResistanceJ is not so much a resistance calculation since it accounts for the resistive effects (when using the Eddy current solver). Rather, it corresponds to the resistance that the circuit would need in order to get the same Joule heating in the context of a circuit equation. If all EM fields are diffused or the RH solver is being used, ResistanceJ should be close to ResistanceD. 4. Only the mutual inductances between the first three circuits defined are output. *EM_DATABASE_CIRCUIT0D Purpose: This keyword enables the output of EM data for every circuit defined. Output options card Card 1 1 2 3 4 5 6 7 8 Variable OUTLV DTOUT Type Default I 0 F 0. VARIABLE DESCRIPTION OUTLV Determines if the output file should be dumped. EQ.0: No output file is generated. EQ.1: The output file is generated. DTOUT Time interval to print the output. If DTOUT is equal to 0.0, then the EM timestep will be used. Remarks: 1. The file name for this database is em_circuit0D_XXX.dat with XXX the circuit ID. 2. At the start of the run, based on the initial values of the meshes resistances and inductances, the solver will calculate the results for a so-called “0D” solution which does not take into account the current’s diffusion, the part’s displacements or the EM material property changes. It is therefore a crude approximation. This can be useful in some cases especially in R,L,C circuits if the users wishes to have an first idea of how the source current will behave. 3. Since the calculation of this 0D circuit can take time depending on the problems size, it should only be used in cases where the output results are useful to the comprehension of the analysis. 4. This card has no influence on the results of the EM run itself. *EM Purpose: This keyword enables the output of EM data on elements. Output Options Card. Card 1 1 2 3 4 5 6 7 8 Variable OUTLV DTOUT Type Default I 0 F 0. Include as many cards as needed. This input ends at the next keyword (“*”) card. Card 2 1 2 3 4 5 6 7 8 Variable ELSID Type I Default none VARIABLE DESCRIPTION OUTLV Determines if the output file should be dumped. EQ.0: No output file is generated. EQ.1: The output file is generated. DTOUT Time interval to print the output. If DTOUT is equal to 0.0, then the EM timestep will be used. ELSID Solid Elements Set ID. Remarks: 1. The file name for this database is em_elout.dat. *EM_DATABASE_FIELDLINE Purpose: The EM solver uses a BEM method to calculate the EM fields between conductors. With this method, the magnetic field in the air or vacuum between conductors is therefore not explicitly computed. However, in some cases, it may be interesting to visualize some magnetic field lines for a better analysis. This keyword allows the output of field line data. It has no influence on the results of the EM solve. Output Options Card. Card 1 1 2 3 4 5 6 7 8 Variable FLID PSID DTOUT NPOINT Type I I F I Default none none 0. 100 Remaining cards are optional.† Card 2 1 Variable INTEG Type Default I 2 2 H F 3 4 5 6 7 8 HMIN HMAX TOLABS TOLREL F F F F 0. 0. 1E10 1E-3 1E-5 Card 3 1 2 3 4 5 6 7 8 Variable BTYPE Type Default I VARIABLE DESCRIPTION FLID PSID Field line set ID Point Set ID associated to the field line set . The coordinates given by the different points will be the starting points of the field lines. DTOUT Time interval to print the output. If DTOUT is equal to 0.0, then the EM time step will be used. NPOINT Number of points per field line. The points are regularly spaced. INTEG Type of numerical integrator used to compute the field lines : EQ.1: RK4, Runge Kutta 4. See Remark 2. EQ.2: DOP853, Dormand Prince 8(5,3). See Remark 2. Value of the step size. In case of an integrator with adaptive step size, it is the initial value of the step size. Minimal step size value. Only used in the case of an integrator with adaptive step size. Maximal step size value. Only used in the case of an integrator with adaptive step size. Absolute tolerance of the integrator. Only used in the case of an integrator with adaptive step size. Relative tolerance of the integrator. Only used in the case of an integrator with adaptive step size. H HMIN HMAX TOLABS TOLREL BTYPE Method to compute the magnetic field : EQ.1: Direct method (every contribution is computed by the Biot Savart Law and summed up : very slow). EQ.2: Multipole method (approximation of the direct method using the multipole expansion). EQ.3: Multicenter method (approximation of the direct method using a weighted subset of points only in order to compute the magnetic field). *EM_DATABASE_FIELDLINE 1. File Names. The file name for this database is em_fieldLine_XX_YYY.dat where XX is the field line ID and YYY is the point set ID defined in *EM_POINT_SET. 2. Integrators. The Runge Kutta 4 integrator is an explicit iterative method for solving ODEs. It is a fourth order method with a constant step size. The Dormand Prince 8(5,3) integrator is an explicit iterative method for solving IDEs. Particular- ly, this integrator is an embedded Runge Kutta integrator of order 8 with an adap- tive step size. This integrator allows a step size control which is done though an error estimate at each step. The Dormand Prince 8(5,3) is a Dormand Prince 8(6) for which the 6th order error estimator has been replaced by a 5th order estimator with 3rd order correction in order to make the integrator more robust. Purpose: This keyword enables the output of global EM. Output Options Card. *EM Card 1 1 2 3 4 5 6 7 8 Variable OUTLV DTOUT Type Default I 0 F 0. VARIABLE DESCRIPTION OUTLV Determines if the output file should be dumped. EQ.0: No output file is generated. EQ.1: The output file is generated. DTOUT Time interval to print the output. If DTOUT is equal to 0.0, then the EM timestep will be used. Remarks: 1. The file name for this database is em_globEnergy.dat. 2. Outputs the global EM energies of the mesh, the air and the source circuit. Also outputs the global kinetic energy and the global plastic work energy. *EM_DATABASE_NODOUT Purpose: This keyword enables the output of EM data on nodes. Output Options Card. Card 1 1 2 3 4 5 6 7 8 Variable OUTLV DTOUT Type Default I 0 F 0. Include as many cards as needed. This input ends at the next keyword (“*”) card. Card 2 1 2 3 4 5 6 7 8 Variable NSID Type I Default none VARIABLE DESCRIPTION OUTLV Determines if the output file should be dumped. EQ.0: No output file is generated. EQ.1: The output file is generated. DTOUT Time interval to print the output. If DTOUT is equal to 0.0, then the EM timestep will be used. NSID Node Set ID. Remarks: 1. The file name for this database is em_nodout.dat. *EM Purpose: This keyword enables the output of EM data for every part defined. . Output Options Card. Card 1 1 2 3 4 5 6 7 8 Variable OUTLV DTOUT Type Default I 0 F 0. VARIABLE DESCRIPTION OUTLV Determines if the output file should be dumped. EQ.0: No output file is generated. EQ.1: The output file is generated. DTOUT Time interval to print the output. If DTOUT is equal to 0.0, then the EM timestep will be used. Remarks: 1. The file name for this database is em_partData_XXX.dat with XXX the part ID. 2. Outputs the part EM energies of the part as well as the Lorentz force. Also outputs the part kinetic energy and the part plastic work energy. *EM_DATABASE_POINTOUT Purpose: This keyword enables the output of EM data on points sets. Output Options Card. Card 1 1 2 3 4 5 6 7 8 Variable OUTLV DTOUT Type Default I 0 F 0. Include as many cards as needed. This input ends at the next keyword (“*”) card. Card 2 1 2 3 4 5 6 7 8 Variable PSID Type I Default none VARIABLE DESCRIPTION OUTLV Determines if the output file should be dumped. EQ.0: No output file is generated. EQ.1: The output file is generated. DTOUT Time interval to print the output. If DTOUT is equal to 0.0, then the ICFD timestep will be used. PSID Point Set ID . Remarks: 1. The file name for this database is em_pointout.dat. *EM Purpose: This keyword enables the output of EM data for every circuit defined. . Output Options Card. Card 1 1 2 3 4 5 6 7 8 Variable OUTLV DTOUT Type Default I 1 F 0. VARIABLE DESCRIPTION OUTLV Determines if the output file should be dumped. EQ.0: No output file is generated. EQ.1: The output file is generated. DTOUT Time interval to print the output. If DTOUT is equal to 0.0, then the EM timestep will be used. Remarks: 1. The file name for this database is em_rogoCoil_XXX.dat where XXX is the rogo Coil ID. *EM_DATABASE_TIMESTEP Purpose: This keyword enables the output of EM data regarding the EM timestep. Output options card. Card 1 1 2 3 4 5 6 7 8 Variable OUTLV Type Default I 0 VARIABLE DESCRIPTION OUTLV Determines if the output file should be dumped. EQ.0: No output file is generated. EQ.1: The output file is generated. Remarks: 1. The file name for this database is em_timestep.dat. 2. Outputs the run’s EM tim estep versus the time step calculated using the EM CFL condition as criteria (autotimestep). This can be useful in cases with big defor- mations and/or material property changes and a fixed time step is being used in case that time step becomes to big compared to the stability time step. *EM Purpose: Define the parameters for a Burgess model giving the electrical conductivity as as a function of the temperature and the density, see: T.J. Burgess, “Electrical resistivity model of metals”, 4th International Conference on Megagauss Magnetic-Field Generation and Related Topics, Santa Fe, NM, USA, 1986 Card 1 1 Variable EOSID Type I 2 V0 F 3 4 GAMMA THETA F F 5 LF F 6 C1 F 7 C2 F 8 C3 F Default none none none none none none none none Card 2 Variable 1 C4 Type F 2 K F 3 4 5 6 7 8 EXPON LGTUNIT TIMUNIT TEMUNI ADJUST I F F I I Default none none none none none none none In the following, UUS stands for User Units System and BUS for Burgess Units VARIABLE DESCRIPTION EOSID ID of the EM_EOS (specified by an *EM_MAT card) V0 Reference specific volume V0 (UUS). GAMMA0 Reference Gruneisen value γ0.(no units). THETA Reference melting temperature θm,0 in eV (BUS). LF C1 C2 Latent heat of fusion LF in kJoule/mol (BUS). C1 constant (BUS) C2 constant (no units) VARIABLE DESCRIPTION C3 C4 K C3 constant (no units) C4 constant (no units) Parameter k (no units). EXPON Exponent in equations (2) LGTUNIT Length units for UUS (relative to meter, i.e. = 1.e-3 if UUS in mm). TIMUNIT Time units for UUS (relative to seconds). TEMUNIT Temperature units EQ.1: temperature in Celsius EQ.2: temperature in Kelvins ADJUST Conductivity modification EQ.0: (default) The conductivity is given by the Burgess formula. EQ.1: The conductivity is adjusted so that it is equal to the conductivity defined in *EM_MAT card σmat at room tem- perature: σ(θ) = σBurgess(θ) σmat σBurgess(θroom) Remarks: 1. The Burgess model gives the electrical resistivity vs temperature and density for the solid phase, liquid phase and vapor phase. At this time, only the solid and liquid phases are implemented. To check which elements are in the solid and in the liquid phase, a melting temperature is first computed by: θ𝑚 = θ𝑚,0 ( 𝑉0 −1 ) (2γ0−1)(1− 𝑉 𝑉0 ) If T < 𝜃𝑚: solid phase model applies. a) The solid phase electrical resistivity corresponds to the Meadon model: η𝑆 = (𝐶1 + 𝐶2θ𝐶3)𝑓𝑐 ( 𝑉0 ), (1) where θ is the temperature, V is the specific volume, and V0 is the reference specific volume (zero pressure, solid phase). In (1), the volume dependence is given by: 2γ−1 2γ+1 2γ ) ) ) EXPON.EQ. −1 (most materials) EXPON.EQ. +1 (tungsten) EXPON.EQ. 0 (stainless steel) ( ( ( 𝑉0 𝑉0 𝑉0 ⎧ { { { { { ⎨ { { { { { ⎩ 𝑓𝑐 ( 𝑉0 ) = with γ = γ0 − (γ0 − ) (1 − 𝑉0 ) b) If T > θm : liquid phase model: η𝐿 = (η𝐿)θ𝑚 ( θ𝑚 𝐶4 ) (η𝐿)θ𝑚 = Δη(η𝑆)θ𝑚 with where (2) (3) (4) Δ𝜂 = ⎧𝑘𝑒0.69𝐿𝐹/θ𝑚 {{ ⎨ {{ ⎩ 1 + 0.0772(2 − θ𝑚) 1 + 0.106(0.846 − θ𝑚) 𝑘 > 0 𝑘 = −1 (tungsten) (5) 𝑘 = −2 (stainless steel SS-304) The following table reports some sets of parameters given by Burgess in his paper: Parameter Cu Ag Au W Al(2024) SS(304) V0(cm3/gm) 0.112 0.0953 0.0518 0.0518 0.370 0.1265 γ0 θm,0 (BUS) 2.00 2.55 3.29 1.55 2.13 2.00 0.117 0.106 0.115 0.315 0.0804 0.156 LF (BUS) 0.130 0.113 0.127 0.337 0.107 0.153 C1 (BUS) -4.12e-5 -3.37e-5 -4.95e-5 -9.73e-5 -5.35e-5 0 C2 C3 0.113 0.131 0.170 0.465 0.233 0.330 1.145 1.191 1.178 1.226 1.210 0.4133 EXPON -1 -1 -1 +1 -1 Parameter Cu Ag Au W Al(2024) SS(304) C4 k 0.700 0.672 0.673 0.670 0.638 0.089 0.964 0.910 1.08 -1. 0.878 -2. *EM Purpose: Define the parameters for a Meadon model, giving the electrical conductivity as a function of the temperature and the density; see: T.J. Burgess, “Electrical resistivity model of metals”, 4th International Conference on Megagauss Magnetic-Field Generation and Related Topics, Santa Fe, NM, USA, 1986 Card 1 1 Variable EOSID Type I 2 C1 F 3 C2 F 4 C3 F 5 TEMUNI I 6 V0 F 7 8 GAMMA EXPON F I Default none none none none none none none none Card 2 1 2 3 4 5 6 7 8 Variable LGTUNIT TIMUNIT ADJUST Type F F I Default none none none In the following, UUS stands for User Units System and BUS for Burgess Units. VARIABLE DESCRIPTION EOSID ID of the EM_EOS C1 C2 C3 C1 constant (BUS) C2 constant (no units) C3 constant (no units) TEMUNIT Temperature units EQ.1: temperature in Celsius EQ.2: temperature in Kelvins VARIABLE DESCRIPTION V0 Reference specific volume V0 (UUS). GAMMA0 Reference Gruneisen value γ0.(no units). EXPON Exponent in equations (7) LGTUNIT Length units for UUS (relative to meter, i.e. = 1.e-3 if UUS in mm). TIMUNIT Time units for UUS (relative to seconds). ADJUST: EQ.0: (default) the conductivity is given by the Burgess formula. EQ.1: The conductivity is adjusted so that it is equal to the conductivity defined in the *EM_MAT card σmatat room temperature: σ(θ) = σBurgess(θ) σmat σBurgess(θroom) Remarks: 1. The Meadon model is a simplified Burgess model with the solid phase equations only. The electrical resistivity is given by: η𝑆 = (𝐶1 + 𝐶2θ𝐶3)𝑓𝑐 ( 𝑉0 ) (6) where θ is the temperature, V is the specific volume, and V0 is the reference specif- ic volume (zero pressure, solid phase). In (6), the volume dependence is given by: 𝑓𝑐 ( 𝑉0 ) = ⎧ { { { { { { ⎨ { { { { { { ⎩ 2γ−1 2γ+1 2γ ) ) ) EXPON.EQ. −1 (most materials) EXPON.EQ. +1 (tungsten) (7) EXPON.EQ.0 (stainless steel) ( ( ( 𝑉0 𝑉0 𝑉0 VO.EQ. 0 (default value for 𝑉0 is zero) (In this last case, only EOSID, C1, C2, C3, TEMUNIT, TIMUNIT and LGTUNIT need to be defined) with, ) (1 − 𝑉0 ) *EM (8) The following table reports some sets of parameters given by Burgess in his paper: Parameter Cu Ag Au W Al(2024) SS(304) V0(cm3/gm) 0.112 0.0953 0.0518 0.0518 0.370 0.1265 γ0 2.00 2.55 3.29 1.55 2.13 2.00 C1 (BUS) -4.12e-5 -3.37e-5 -4.95e-5 -9.73e-5 -5.35e-5 0 C2 C3 0.113 0.131 0.170 0.465 0.233 0.330 1.145 1.191 1.178 1.226 1.210 0.4133 EXPON -1 -1 -1 +1 -1 *EM_EOS_PERMEABILITY Purpose: Define the parameters for the behavior of a material’s permeability Card 1 1 2 3 4 5 6 7 8 Variable EOSID EOSTYPE LCID Type I I I Default none none none VARIABLE DESCRIPTION EOSID ID of the EM_EOS EOSTYPE Define the type of EOS: EQ.1: Permeability defined by a B function of H curve (B = µH) EQ.2: Permeability defined by a H function of B curve (H = B/µ) LCID Load curve ID *EM Purpose: Define the electrical conductivity as a function of temperature by using a load curve. Card 1 1 2 3 4 5 6 7 8 Variable EOSID LCID Type I I Default none none VARIABLE DESCRIPTION EOSID ID of the EM_EOS LCID Load curve ID. Remarks: 1. The load curve describes the electrical conductivity (ordinate) vs the temperature (abscissa). The user needs to make sure the temperature and the electrical conduc- tivity given by the load curve are in the correct units. Also, it is advised to give some bounds to the load curve (conductivities at very low and very high tempera- tures) to avoid bad extrapolations of the conductivity if the temperature gets out of the load curve bounds. *EM_EOS_TABULATED1 Purpose: Define the electrical conductivity as a function of time by using a load curve. Card 1 1 2 3 4 5 6 7 8 Variable EOSID LCID Type I I Default none none VARIABLE DESCRIPTION EOSID ID of the EM_EOS LCID Load curve ID. Remarks: 1. The load curve describes the electrical conductivity (ordinate) vs the time (abscissa). The user needs to make sure the time and the electrical conductivity given by the load curve are in the correct units. Also, it is advised to give some bounds to the load curve (conductivities at t = 0 at after a long time) to avoid bad extrapolations of the conductivity if the run time gets out of the load curve bounds. 2. LCID can also refer to a DEFINE FUNCTION. If a DEFINE_FUNCTION is used, allowed: the 𝑓 (𝑣𝑥, 𝑣𝑦, 𝑣𝑧, 𝑡𝑒𝑚𝑝, 𝑝𝑟𝑒𝑠, 𝑣𝑜𝑙, 𝑚𝑎𝑠𝑠, 𝐸𝑥, 𝐸𝑦, 𝐸𝑧, 𝐵𝑥, 𝐵𝑦, 𝐵𝑧, 𝐹𝑥, 𝐹𝑦, 𝐹𝑧, 𝐽𝐻𝑟𝑎𝑡𝑒, 𝑡𝑖𝑚𝑒). 𝐹𝑥, 𝐹𝑦, 𝐹𝑧 refers to the Lorentz force vector. parameters following are *EM Purpose: Define the components of a time dependent exterior field uniform in space applied on the conducting parts. Card 1 1 2 3 4 5 6 7 8 Variable FIELDID FTYPE FDEF LCIDX LCIDY LCIDZ Type Default I 0 I 0 F 0 I 0 I 0 I 0 VARIABLE DESCRIPTION FIELDID External Field ID FTYPE Field type: EQ.1: Magnetic field EQ.2: Electric field (not available yet) FDEF Field defined by : EQ.1: Load Curves LCID[X,Y,Z] Load curve ID defining the (X,Y,Z) component of the field function of time *EM_EXTERNAL_FIELD Purpose: Defining an isopotential, i.e. constrain nodes so that they have the same scalar potential value. This card is to be used with the EM solver of type 3 and the distributed Randle circuits only at this time. Card 1 1 2 3 4 5 6 7 8 Variable ISOID SETTYPE SETID Type I I I Default none none none VARIABLE DESCRIPTION ISOID ID of the Isopotential SETTYPE Set type: EQ.2: Node Set. SETID Set ID Purpose: Define a connection between two isopotentials. *EM Card 1 1 2 3 4 5 6 7 8 Variable CONID CONTYPE ISOID1 ISOID2 VAL LCID Type I I I I F I Default none none none none none none VARIABLE DESCRIPTION CONID Connection ID CONTYPE Connection type : EQ.1: Short Circuit. EQ.2: Resistance. EQ.3: Voltage Source. EQ.4: Current Source. ISOID1 ID of the first isopotential to be connected ISOID2 ID of the second isopotential to be connected VAL LCID Value of the resistance, voltage or current depending on CONTYPE Ignored if LCID defined. Load curve ID defining the value of the resistance, voltage or current function of time and depending on CONTYPE. If not defined, VAL will be used. *EM_MAT_001 Purpose: Define the electromagnetic material type and properties for a material whose permeability equals the free space permeability. Include as many cards as needed. This input ends at the next keyword (“*”) card. Card 1 1 2 3 4 5 6 7 8 Variable MID MTYPE SIGMA EOSID Type I I F I Default none none none none VARIABLE DESCRIPTION MID Material ID: refers to MID in the *PART card. MTYPE Defines the electromagnetism type of the material: EQ.0: Air or vacuum EQ.1: Insulator material. these materials have the same electromagnetism behavior as EQ.0 EQ.2: Conductor carrying a source. In these conductors, the eddy current problem is solved, which gives the actual current density. Typically, this would correspond to the coil. EQ.4: Conductor not connected to any current or voltage source, where the Eddy current problem is solved. Typically, this would correspond to the workpiece SIGMA Initial electrical conductivity of the material EOSID ID of the EOS to be used for the electrical conductivity . *EM Purpose: Define an electromagnetic material type and properties whose permeability is different than the free space permeability. Include as many cards as needed. This input ends at the next keyword (“*”) card. Card 1 1 2 3 4 5 6 7 8 Variable MID MTYPE SIGMA EOSID MUREL EOSMU Type I I F I F I Default none none none none none none VARIABLE DESCRIPTION MID Material ID: refers to MID in the *PART card. MTYPE Defines the electromagnetism type of the material: EQ.0: Air or vacuum EQ.1: Insulator material. These materials have the same electromagnetism behavior as EQ.0 EQ.2: Conductor carrying a source. In these conductors, the eddy current problem is solved, which gives the actual current density. Typically, this would correspond to the coil. EQ.4: Conductor not connected to any current or voltage source, where the Eddy current problem is solved. Typically, this would correspond to the workpiece SIGMA Initial electrical conductivity of the material EOSID MUREL EOSMU ID of the EOS to be used for the electrical conductivity . Relative permeability: Is the ratio of the permeability of a specific medium to the permeability of free space (𝜇𝑟 = 𝜇/𝜇0) ID of the EOS to be used to define the behavior of µ by an equation of state (Note: if EOSMU is defined, MUREL will be used for the initial value only). *EM_MAT_002 Purpose: Define an electromagnetic material type whose electromagnetic conductivity is defined by a (3*3) tensor matrix. Applications include composite materials. Orthotropic Card 1. Card 1 1 2 3 4 5 6 7 8 Variable MID MTYPE SIGMA11 SIGMA22 SIGMA33 Type I I F F F Orthotropic Card 2. Card 2 1 2 3 4 5 6 7 8 Variable SIGMA12 SIGMA13 SIGMA21 SIGMA23 SIGMA31 SIGMA32 AOPT Type F F F F F F I Orthotropic Card 3. Card 1 Variable 1 XP Type F Orthotropic Card 4. Card 2 Variable 1 V1 Type F 2 YP F 2 V2 F 7 8 MACF I 7 8 3 ZP F 3 V3 F 4 A1 F 4 D1 5 A2 F 5 D2 6 A3 F 6 D3 F F F VARIABLE DESCRIPTION MID Material ID: refers to MID in the *PART card. MTYPE Defines the electromagnetism type of the material: EQ.0: Air or vacuum EQ.1: Insulator material: These materials have electromagnetism behavior as EQ.0 the same EQ.2: Conductor carrying a source. In these conductors, the eddy current problem is solved, which gives the actual current density. Typically, this would correspond to the coil. EQ.4: Conductor not connected to any current or voltage source, where the Eddy current problem is solved. Typically, this would correspond to the workpiece. SIGMA11 SIGMA12 The 1, 1 term in the 3 × 3 electromagnetic conductivity tensor matrix. Note that 1 corresponds to the a material direction The 1, 2 term in the 3 × 3 electromagnetic conductivity tensor matrix. Note that 2 corresponds to the b material direction ⋮ ⋮ SIGMA33 The 3, 3 term in the 3 × 3 electromagnetic conductivity tensor matrix. Define AOPT for both options: AOPT Material axes option, see the figure in *MAT_002. EQ.0.0: locally orthotropic with material axes determined by element nodes as shown in part (a) the figure in *MAT_002. The a-direction is from node 1 to node 2 of the element. The b-direction is orthogonal to the a- direction and is in the plane formed by nodes 1, 2, and 4. EQ.1.0: locally orthotropic with material axes determined by a point in space and the global location of the element cen- ter; this is the a-direction. EQ.2.0: globally orthotropic with material axes determined by vectors defined below, as with *DEFINE_COORDI- NATE_VECTOR. EQ.3.0: locally orthotropic material axes determined by rotating the material axes about the element normal by an angle, BETA, from a line in the plane of the element defined by the cross product of the vector v with the element nor- mal. The plane of a solid element is the midsurface be- tween the inner surface and outer surface defined by the first four nodes and the last four nodes of the connectivi- ty of the element, respectively. EQ.4.0: locally orthotropic in cylindrical coordinate system with the material axes determined by a vector v, and an origi- nating point, P, which define the centerline axis. This op- tion is for solid elements only. EQ.5.0: globally defined reference frame with (a,b,c)=(X0,Y0,Z0). XP, YP, ZP Define coordinates of point p for AOPT = 1 and 4. A1, A2, A3 Define components of vector a for AOPT = 2. MACF Material axes change flag for solid elements: EQ.1: No change, default, V1, V2, V3 Define components of vector v for AOPT = 3 and 4. D1, D2, D3 Define components of vector d for AOPT = 2. Remarks: This card works in a similar way to *MAT_002. The procedure for describing the principle material directions is explained for solid elements for this material model. We will call the material direction the a-b-c coordinate system. The AOPT options illustrated in the AOPT figure of *MAT_002 can define the a-b- c system for all elements of the parts that use the material. *EM Purpose: Define the electromagnetic material type and properties for conducting shells in a 3D problem. Include as many cards as needed. This input ends at the next keyword (“*”) card. Card 1 1 2 3 4 5 6 7 8 Variable MID MTYPE SIGMA EOSID NELE Type I I F I Default none none none none I 1 VARIABLE DESCRIPTION MID Material ID: refers to MID in the *PART card. MTYPE Defines the electromagnetism type of the material: EQ.0: Air or vacuum EQ.1: Insulator material. these materials have the same electromagnetism behavior as EQ.0 EQ.2: Conductor carrying a source. In these conductors, the eddy current problem is solved, which gives the actual current density. Typically, this would correspond to the coil. EQ.4: Conductor not connected to any current or voltage source, where the Eddy current problem is solved. Typically, this would correspond to the workpiece SIGMA Initial electrical conductivity of the material EOSID NELE ID of the EOS to be used for the electrical conductivity . Number of elements in the thickness of the shell. It is up to the user to make sure his mesh is fine enough to correctly capture the inductive-diffusive effects . *EM_OUTPUT Purpose: Define the level of EM related output on the screen and in the messag file. Card 1 1 2 3 4 5 6 7 8 Variable MATS MATF SOLS SOLF MESH MEM TIMING Type Default I 0 I 0 I 0 I 0 I 0 I 0 I 0 VARIABLE DESCRIPTION MATS Level of matrix assembly output to the screen: EQ.0: No output EQ.1: Basic assembly steps EQ.2: Basic assembly steps+percentage completed+final statistics EQ.3: Basic assembly steps+percentage completed+statistics at each percentage of completion MATF Level of matrix assembly output to the messag file: EQ.0: No output EQ.1: Basic assembly steps EQ.2: Basic assembly steps+percentage completed+final statistics EQ.3: Basic assembly steps+percentage completed+statistics at each percentage of completion SOLS Level of solver output on the screen: EQ.0: No output EQ.1: Global information at each FEM iteration EQ.2: Detailed information at each FEM iteration DESCRIPTION *EM SOLF Level of solver output to the messag file: EQ.0: No output EQ.1: Global information at each FEM iteration EQ.2: Detailed information at each FEM iteration MESH Controls the output of the mesh data to the d3hsp file EQ.0: No mesh output EQ.1: Mesh info is written to the d3hsp file MEMORY Controls the output of information about the memory used by the EM solve to the messag file: EQ.0: no memory information written. EQ.1: memory information written. TIMING Controls the output of information about the time spent in the different parts of the EM solver to the messag file EQ.0: no timing information written. EQ.1: timing information written. *EM_OUTPUT Purpose: This keyword creates a set of points which can be used by the *EM_DATA- BASE_POINTOUT keyword. Output Options Card. Card 1 1 2 Variable PSID PSTYPE Type Default I 0 I 0 3 VX F 0. 4 VY F 0. 5 VZ F 0. 6 7 8 Include as many cards as needed. This input ends at the next keyword (“*”) card. 5 6 7 8 Card 2 1 Variable PID Type I 2 X F 3 Y F 4 Z F Default none none none none VARIABLE DESCRIPTION PSID Point Set ID. PSTYPE Point Set type : EQ.0: Fixed points. EQ.1: Tracer points using prescribed velocity. VX, VY, VZ Constant velocities to be used when PSTYPE = 1 PID Point ID X, Y, Z Point initial coordinates *EM Purpose: For battery cell internal short, define conditions to turn on a Randle short (replace one or several randle circuits by resistances), and to define the value of the short resistance. Card 1 1 2 3 4 5 6 7 8 Variable AREATYPE FUNCID Type I I Default none none VARIABLE DESCRIPTION AREATYPE Works the same way as RDLAREA in *EM_CIRCUIT_RANDLE : EQ.0: The resistance in FUNCTIONID is taken as is in each Randle circuit. EQ.1: The resistance in FUNCTIONID is per unit area. EQ.2: The resistance in FUNCTIONID is for the whole unit cell (the whole cell is shorted), and then a factor based on ar- eaLocal/areaGlobal is applied. FUNCTIONID DEFINE_FUNCTION ID giving the local resistance function of local parameters for the local randle circuit. Accepted values are: 𝑓 (𝑥𝑐𝑐𝑝, 𝑦𝑐𝑐𝑝, 𝑧𝑐𝑐𝑝, 𝑥𝑠𝑒𝑝, 𝑦𝑠𝑒𝑝, 𝑧𝑠𝑒𝑝, 𝑥𝑠𝑒𝑚, 𝑦𝑠𝑒𝑚, 𝑧𝑠𝑒𝑚, 𝑥𝑐𝑐𝑚, 𝑦𝑐𝑐𝑚, 𝑧𝑐𝑐𝑚, 𝑡𝑖𝑚𝑒). Remarks: 1. If the return value of the function is negative, there is no short, the randle circuit is maintained. If it is negative, the function gives the value of the reistance. 2. The parameter description is : a) x_ccp: x of boundary between positive current collector and positive elec- trode b) x_sep: x of boundary between positive electrode and separator c) x_sem: x of boundary between separator and negative electrode d) x_ccm: x of boundary between negative electrode and negative current col- lector 3. An example of a function : *DEFINE_FUNCTION FID (Function Id) Float resistance_short_randle( float time, float x_ccp,float y_ccp,float z_ccp, float x_sep,float y_sep,float z_sep, float x_sem,float y_sem,float z_sem, float x_ccm,float y_ccm,float z_ccm) { float seThick0; seThick0 = 1.e-5; seThick=(sqrt(x_sep-x_sem)^2+(y_sep-y_sem)^2+(z_sep-z_sem)^2); if (seThick >= seThick0) then return -1; else return 1.e-2; endif *EM Purpose: Define a rotation axis for the EM solver. This is used with the 2D axisymmetric solver. The axis is defined by a point and a direction. Card 1 Variable 1 XP Type F 2 YP F 3 ZP F 4 XD F 5 YD F 6 7 8 ZD NUMSEC F I Default none none none none none none none VARIABLE DESCRIPTION XP, YP, ZP 𝑥, 𝑦, and 𝑧 coordinates of the point XD, YD, ZD 𝑥, 𝑦, and 𝑧 components of direction of the axis NUMSEC Number of Sectors. This field gives the ratio of the full circle to the angular extension of the mesh. This has to be a power of two. For example, NUMSEC = 4 means that the mesh of the part represents one fourth of the total circle. If NUMSEC = 0 for *EM_2DAXI, the solver will replace it with this value. *EM_SOLVER_BEM Purpose: Define the type of linear solver and pre-conditioner as well as tolerance for the EM_BEM solve. Card 1 1 2 3 4 5 6 7 8 Variable RELTOL MAXITE STYPE PRECON USELAS NCYCLBEM Type I I Default 1E-6 1000 I 2 I 2 I 1 I 5000 VARIABLE RELTOL DESCRIPTION Relative tolerance for the iterative solvers (PCG or GMRES). The user should try to decrease this tolerance if the results are not accurate enough. More iterations will then be needed. MAXITER Maximal number of iterations. STYPE Solver type: EQ.1: Direct solve – the matrices will then be considered as dense. EQ.2: Pre-Conditioned Gradient method (PCG) - this allows to have block matrices with low rank blocks, and thus reduce memory used. EQ.3: GMRES method - this allows to have block matrices with low rank blocks and thus reduce memory used. The GMRES option only works in Serial for now. PRECON Preconditioner type for PCG or GMRES iterative solves: EQ.0: No preconditioner EQ.1: Diagonal line EQ.2: Diagonal block EQ.3: Broad diagonal including all neighbor faces EQ.4: LLT factorization. The LLT factorization option only works in serial for now. VARIABLE DESCRIPTION USELAST This is used only for iterative solvers (PCG or GMRES). EQ.-1: Start from 0 as initial guess for solution of the linear system. EQ.1: Starts from the previous solution normalized by the RHS change. NCYLBEM Number of electromagnetism cycles between the recalculation of BEM matrices. Remarks: 1. Using USELAST = 1 can save many iterations in the subsequent solves if the vector solution of the present solve is assumed to be nearly parallel to the vector solution of the previous solve, as usually happens in time-domain eddy-current problems. 2. Since the BEM matrices depend on (and only on) the surface node coordinates of the conductors, it is important to recalculate them when the conductors are mov- ing. The frequency with which they are updated is controlled by NCYLBEM. Note that very small values, for example NCYLBEM = 1, should, generally, be avoided since this calculation involves a high computational cost. However, when two conductors are moving and in contact with each other it is recommended to recalculate the matrices at every time step. *EM_SOLVER_BEMMAT Purpose: Define the type of BEM matrices as well as the way they are assembled. Card 1 1 2 3 4 5 6 7 8 Variable MATID Type I Default none RELTOL F 1E-6 VARIABLE DESCRIPTION MATID Defines which BEM matrix the card refers to: EQ.1: 𝐏 matrix EQ.2: 𝐐 matrix RELTOL Relative tolerance on the sub-blocks of the matrix when doing low rank approximations. The user should try to decrease these tolerances if the results are not accurate enough. More memory will then be needed. *EM Purpose: Define some parameters for the EM_FEM solver. Card 1 1 2 3 4 5 6 7 8 Variable RELTOL MAXITE STYPE PRECON USELAST NCYCLFEM Type I I Default 10-3 1000 I 1 I 1 I 1 I 5000 VARIABLE RELTOL DESCRIPTION Relative tolerance for the iterative solvers (PCG or GMRES). The user should try to decrease this tolerance if the results are not accurate enough. More iterations will then be needed. MAXITER Maximal number of iterations. STYPE Solver type: EQ.1: Direct solve EQ.2: Conditioned Gradient Method (PCG) PRECON Preconditioner type for PCG. EQ.0: No preconditioner EQ.1: Diagonal line USELAST This is used only for iterative solvers (PCG). EQ.-1: starts from 0 as initial solution of the linear system. EQ.1: starts from previous solution normalized by the right- hand-side change change. NCYCLFEM Number of electromagnetism cycles between the recalculation of FEM matrices. *EM_SOLVER_FEM 1. Using USELAST = 1 can save many iterations in the subsequent solves if the vector solution of the present solve is assumed to be nearly parallel to the vector solution of the previous solve, as usually happens in time-domain eddy-current problems. 2. The default values are only valid when the PCG resolution method (STYPE = 2). For the default direct solve (STYPE = 1) those values are ignored. 3. When the conductor parts are deforming or undergoing changes in their EM material properties (conductivity for example), it is important to change the de- fault value of NCYLFEM to recalculate the FEM matrices more often. *EM Purpose: Define some parameters for the coupling between the EM_FEM and EM_BEM solvers. Card 1 1 2 3 4 5 6 7 8 Variable RELTOL MAXITE FORCON Type F I Default 1E-2 50 I 0 VARIABLE RELTOL DESCRIPTION Relative tolerance for the solver. The user should try to decrease this tolerance if the results are not accurate enough. More iterations will then be needed. MAXITER Maximal number of iterations. FORCON EQ.0: the code stops with an error if no convergence EQ.1: the code continues to the next time step even if the RELTOL convergence criteria has not been reached.. *EM_SOLVER_FEMBEM Purpose: Impose a voltage drop between two segment sets. Card 1 1 2 3 4 5 6 7 8 Variable VDID VDTYPE SSID1 SSID2 VOLT Type I I I I F Default none none none none none VARIABLE DESCRIPTION VDID Voltage Drop ID VDTYPE Voltage Drop Type: EQ.1: Voltage drop between the two corresponding nodes of the two segment sets SSID1 and SSID2. SSID1 SSID2 VOLT Segment Set ID 1 Segment Set ID 2 Value of the voltage drop *ICFD The keyword *ICFD covers all the different options available in the incompressible fluid solver. The keyword cards in this section are defined in alphabetical order: *ICFD_BOUNDARY_CONJ_HEAT *ICFD_BOUNDARY_FLUX_TEMP *ICFD_BOUNDARY_FREESLIP *ICFD_BOUNDARY_FSI *ICFD_BOUNDARY_FSWAVE *ICFD_BOUNDARY_GROUND *ICFD_BOUNDARY_NONSLIP *ICFD_BOUNDARY_PRESCRIBED_MOVEMESH *ICFD_BOUNDARY_PRESCRIBED_PRE *ICFD_BOUNDARY_PRESCRIBED_TEMP *ICFD_BOUNDARY_PRESCRIBED_TURBULENCE *ICFD_BOUNDARY_PRESCRIBED_VEL *ICFD_BOUNDARY_WINDKESSEL *ICFD_CONTROL_ADAPT *ICFD_CONTROL_ADAPT_SIZE *ICFD_CONTROL_CONJ *ICFD_CONTROL_DEM_COUPLING *ICFD_CONTROL_FSI *ICFD_CONTROL_GENERAL *ICFD_CONTROL_IMPOSED_MOVE *ICFD_CONTROL_LOAD *ICFD_CONTROL_MESH *ICFD_CONTROL_MESH_MOV *ICFD_CONTROL_MONOLITHIC *ICFD_CONTROL_OUTPUT *ICFD_CONTROL_OUTPUT_SUBDOM *ICFD_CONTROL_PARTITION *ICFD_CONTROL_POROUS *ICFD_CONTROL_STEADY *ICFD_CONTROL_SURFMESH *ICFD_CONTROL_TAVERAGE *ICFD_CONTROL_TIME *ICFD_CONTROL_TRANSIENT *ICFD_CONTROL_TURB_SYNTHESIS *ICFD_CONTROL_TURBULENCE *ICFD_DATABASE_AVERAGE *ICFD_DATABASE_DRAG *ICFD_DATABASE_FLUX *ICFD_DATABASE_HTC *ICFD_DATABASE_NODEAVG *ICFD_DATABASE_NODOUT *ICFD_DATABASE_POINTAVG *ICFD_DATABASE_POINTOUT *ICFD_DATABASE_RESIDUALS *ICFD_DATABASE_TEMP *ICFD_DATABASE_TIMESTEP *ICFD_DATABASE_UINDEX *ICFD_DEFINE_NONINERTIAL *ICFD_DEFINE_POINT *ICFD_DEFINE_WAVE_DAMPING *ICFD_INITIAL *ICFD_INITIAL_TURBULENCE *ICFD_MAT *ICFD_MODEL_NONNEWT *ICFD_MODEL_POROUS *ICFD_PART *ICFD_PART_VOL *ICFD_SECTION *ICFD_SET_NODE *ICFD_SOLVER_SPLIT *ICFD_SOLVER_TOL_MMOV *ICFD_SOLVER_TOL_MOM *ICFD_SOLVER_TOL_MONOLITHIC *ICFD_SOLVER_TOL_PRE *ICFD_SOLVER_TOL_TEMP *ICFD_BOUNDARY_CONJ_HEAT Purpose: Specify which boundary of the fluid domain will exchange heat with the solid. Include as many cards as needed. This input ends at the next keyword (“*”) card. Card 1 1 2 3 4 5 6 7 8 Variable PID Type I Default none VARIABLE DESCRIPTION PID PID of the fluid surface in contact with the solid. *ICFD Purpose: Impose a heat flux on the boundary expressed as 𝑞 = ∇𝑇 Include as many cards as needed. This input ends at the next keyword (“*”) card. Card 1 1 2 Variable PID LCID Type I I 3 SF F 4 5 6 7 8 DEATH BIRTH F F Default none none 1. 1.E+28 0.0 VARIABLE DESCRIPTION PID LCID PID for a fluid surface. *DEFINE_CURVE, Load curve ID to describe the temperature flux value versus time, or see *DEFINE_FUNCTION. . If a DEFINE_FUNCTION is used, the following allowed: 𝑓 (𝑥, 𝑦, 𝑧, 𝑣𝑥, 𝑣𝑦, 𝑣𝑧, 𝑡𝑒𝑚𝑝, 𝑝𝑟𝑒𝑠, 𝑡𝑖𝑚𝑒). *DEFINE_CURVE_FUNCTION parameters are SF Load curve scale factor. (default = 1.0) DEATH Time at which the imposed motion/constraint is removed: EQ.0.0: default set to 10e28 BIRTH Time at which the imposed pressure is activated starting from the initial abscissa value of the curve *ICFD_BOUNDARY_FREESLIP Purpose: Specify the fluid boundary with free-slip boundary condition. Include as many cards as needed. This input ends at the next keyword (“*”) card. Card 1 1 2 3 4 5 6 7 8 Variable PID Type I Default none VARIABLE PID DESCRIPTION PID of the fluid surface where a free-slip boundary condition is applied. *ICFD Purpose: This keyword defines which fluid surfaces will be considered in contact with the solid surfaces for fluid-structure interaction (FSI) analysis. This keyword should not be defined if *ICFD_CONTROL_FSI is not defined. Include as many cards as needed. This input ends at the next keyword (“*”) card. Card 1 1 2 3 4 5 6 7 8 Variable PID Type I Default none VARIABLE DESCRIPTION PID PID of the fluid surface in contact with the solid domain. *ICFD_BOUNDARY_FSWAVE Purpose: Impose a wave inflow boundary condition. Include as many cards as needed. This input ends at the next keyword (“*”) card. Card 1 1 2 3 4 5 6 7 8 Variable PID WTYPE HEIGHT WAMP WLENG WANG SFLCID Type I I F F F F I Default none none none none none none none VARIABLE DESCRIPTION PID PID for a fluid surface. WTYPE Wave Type: EQ.1: Stokes wave of first order EQ.2: Stokes wave of second order HEIGHT Free surface equilibrium level WAMP Wave amplitude WLENG Wave Length WANG Wave Incidence Angle (3D only) SFLCID Scale factor LCID on the wave amplitude *ICFD Purpose: Specify the fluid boundary with a ground boundary condition. The ground boundary condition is similar to the nonslip boundary condition except that it will keep V = 0 in all circumstances, even if the surface nodes are moving. This is useful in cases where (using ICFD_BOUNDARY_PRESCRIBED_MOVEMESH for example) but those displacements are only to accommodate for mesh movement and do not correspond to a physical motion. to move translate allowed nodes the are or Include as many cards as needed. This input ends at the next keyword (“*”) card. Card 1 1 2 3 4 5 6 7 8 Variable PID Type I Default none VARIABLE PID DESCRIPTION PID of the fluid surface where a ground boundary condition is applied. *ICFD_BOUNDARY_NONSLIP Purpose: Specify the fluid boundary with a non-slip boundary condition. Include as many cards as needed. This input ends at the next keyword (“*”) card. Card 1 1 2 3 4 5 6 7 8 Variable PID Type I Default none VARIABLE PID DESCRIPTION PID of the fluid surface where a non-slip boundary condition is applied. *ICFD_BOUNDARY_PRESCRIBED_MOVEMESH Purpose: Allows the node of a fluid surface to translate in certain directions using an ALE approach. This is useful in piston type applications or can also be used in certain cases to avoid big mesh deformation. Include as many cards as needed. This input ends at the next keyword (“*”) card. Card 1 1 2 3 4 5 6 7 8 Variable PID dofx dofy dofz Type I Default none I 1 I 1 I 1 VARIABLE DESCRIPTION PID PID for a fluid surface. dofx, dofy, dofz Degrees of freedom in the X,Y and Z directions : EQ.0: degree of freedom left free (Surface nodes can translate in the chosen direction) EQ.1: prescribed degree of freedom (Surface nodes are blocked) *ICFD_BOUNDARY_PRESCRIBED_PRE Purpose: Impose a fluid pressure on the boundary. Include as many cards as needed. This input ends at the next keyword (“*”) card. Card 1 1 2 Variable PID LCID Type I I 3 SF F 4 5 6 7 8 DEATH BIRTH F F Default none none 1. 1.E+28 0.0 VARIABLE DESCRIPTION PID LCID PID for a fluid surface. Load curve ID to describe the pressure value versus time, see *DE- or FINE_CURVE, *DEFINE_FUNCTION. . If a DEFINE_FUNCTION is used, the following allowed: 𝑓 (𝑥, 𝑦, 𝑧, 𝑣𝑥, 𝑣𝑦, 𝑣𝑧, 𝑡𝑒𝑚𝑝, 𝑝𝑟𝑒𝑠, 𝑡𝑖𝑚𝑒). *DEFINE_CURVE_FUNCTION parameters are SF Load curve scale factor. (default = 1.0) DEATH Time at which the imposed motion/constraint is removed: EQ.0.0: default set to 10E28 BIRTH Time at which the imposed pressure is activated starting from the initial abscissa value of the curve *ICFD_BOUNDARY_PRESCRIBED_TEMP Purpose: Impose a fluid temperature on the boundary. Include as many cards as needed. This input ends at the next keyword (“*”) card. Card 1 1 2 Variable PID LCID Type I I 3 SF F 4 5 6 7 8 DEATH BIRTH F F Default none none 1. 1.E+28 0.0 VARIABLE DESCRIPTION PID LCID PID for a fluid surface. Load curve ID to describe the temperature value versus time; see or *DEFINE_CURVE, *DEFINE_FUNCTION. . If a DEFINE_FUNCTION is used, the following allowed: 𝑓 (𝑥, 𝑦, 𝑧, 𝑣𝑥, 𝑣𝑦, 𝑣𝑧, 𝑡𝑒𝑚𝑝, 𝑝𝑟𝑒𝑠, 𝑡𝑖𝑚𝑒). *DEFINE_CURVE_FUNCTION parameters are SF Load curve scale factor. (default = 1.0) DEATH Time at which the imposed temperature is removed: EQ.0.0: default set to 10E28 BIRTH Time at which the imposed temperature is activated starting from the initial abscissa value of the curve *ICFD_BOUNDARY_PRESCRIBED_TURBULENCE Purpose: Optional keyword that allows the user to strongly impose the turbulence quantities when a RANS turbulence model is selected. See ICFD_CONTROL_TURBU- LENCE. Mainly used to modify the default boundary conditions at the inlet. Include as many cards as needed. This input ends at the next keyword (“*”) card. Card 1 1 2 3 4 5 6 7 8 Variable PID VTYPE IMP LCID Type I I Default none none I 0 I none VARIABLE DESCRIPTION PID PID for a fluid surface. VTYPE Variable type. EQ.1: kinetic turbulent energy EQ.2: turbulent dissipation rate EQ.3: specific dissipation rate EQ.4: modified turbulent viscosity IMP Imposition method. EQ.0: Direct imposition through value specified by LCID EQ.1: Using turbulent Intensity specified by LCID if VTYPE = 1. Using turbulence length scale specified by LCID if VTYPE = 2,3 and 4. EQ.2: Using turbulent viscosity ratio specified by LCID. Only available for VTYPE = 2 and VTYPE = 3. LCID Load curve ID to describe the variable value versus time, see *DE- FINE_CURVE, *DEFINE_CURVE_FUNCTION or *DEFINE_FUNC- TION. . If a DEFINE_FUNCTION is used, the following parameters are allowed: 𝑓 (𝑥, 𝑦, 𝑧, 𝑣𝑥, 𝑣𝑦, 𝑣𝑧, 𝑡𝑒𝑚𝑝, 𝑝𝑟𝑒𝑠, 𝑡𝑖𝑚𝑒, 𝑘, 𝑒, 𝑚𝑢𝑡). Remarks: 1. At the inlet, the relationship between the turbulent kinetic energy 𝑘 and the turbulence intensity 𝐼 is given by : 𝑘 = (𝑈𝑎𝑣𝑔 2𝐼2) By default, the solver uses an inlet intensity of 0.05 (5%). 2. At the inlet, if specifying the turbulent dissipation rate using a length scale, 𝑙, the following relationship will be used : 𝜖 = 𝐶𝜇 3/4 𝑘3/2 By default, the solver estimates a length scale based on the total height of the chan- nel. Otherwise, if using the turbulent viscosity ratio 𝑟 = 𝜇𝑡 𝜇 method: 𝜖 = 𝜌𝐶𝜇 𝑘2 𝜇 𝑟 3. At the inlet, if specifying the specific dissipation rate using a length scale, 𝑙, the following relationship will be used : 𝜔 = 𝐶𝜇 −1/4 𝑘1/2 By default, the solver estimates a length scale based on the total height of the chan- nel. Otherwise, if using the turbulent viscosity ratio 𝑟 = 𝜇𝑡 𝜇 method: LS-DYNA R10.0 5-15 (ICFD) 𝜔 = 𝜌 4. At the inlet, the relationship between the modified turbulent viscosity 𝜈̃ is given and the length scale, 𝑙 is given by : 𝜈̃ = 0.05√ (𝑈𝑎𝑣𝑔 𝑙) *ICFD_BOUNDARY_PRESCRIBED_VEL Purpose: Impose the fluid velocity on the boundary. Include as many cards as needed. This input ends at the next keyword (“*”) card. Card 1 1 2 3 4 Variable PID DOF VAD LCID Type I I Default none none I 1 I none 1. 5 SF F 6 7 8 VID DEATH BIRTH I 0 F F 1.E+28 0.0 VARIABLE DESCRIPTION PID DOF PID for a fluid surface. Applicable degrees of freedom: EQ.1: 𝑥- degree of freedom, EQ.2: 𝑦- degree of freedom, EQ.3: 𝑧 degree of freedom, EQ.4: Normal direction degree of freedom, VAD Velocity flag: EQ.1: Linear velocity EQ.2: Angular velocity EQ.3: Parabolic velocity profile EQ.4: Activates synthetic turbulent field on part. See *ICFD_- CONTROL_TURB_SYNTHESIS. Load curve ID used to describe motion value versus time, see *DE- FINE_CURVE, *DEFINE_CURVE_FUNCTION, or *DEFINE_FUNC- TION. If a DEFINE_FUNCTION is used, the following parameters are allowed: 𝑓 (𝑥, 𝑦, 𝑧, 𝑣𝑥, 𝑣𝑦, 𝑣𝑧, 𝑡𝑒𝑚𝑝, 𝑝𝑟𝑒𝑠, 𝑡𝑖𝑚𝑒). Load curve scale factor. (default = 1.0) Point ID for angular velocity application point, see *ICFD_DE- FINE_POINT. LCID SF VID *ICFD_BOUNDARY_PRESCRIBED_VEL DESCRIPTION DEATH Time at which the imposed motion/constraint is removed: EQ.0.0: default set to 1028 BIRTH Time at which the imposed motion/constraint is activated starting from the initial abscissa value of the curve *ICFD Purpose: This boundary condition imposes the pressure function of circuit parameters where an analogy is made between the pressure and scalar potential as well as between the flux and the current intensity. Such conditions are frequently encountered in hemodynam- ics. Card 1 1 2 Variable PID WTYPE Type I I 3 R1 F Default none none 0. 4 C1 F 0. 5 R2 F 0. 6 L1 F 0. 7 8 4 5 6 7 8 Optional card if WTYPE = 3 or 4. Card 2 1 Variable P2LCID Type I 2 C2 F Default None 0. 3 R3 F 0. VARIABLE DESCRIPTION PID PID for a fluid surface WTYPE Circuit type : EQ.1: Windkessel circuit EQ.2: Windkessel circuit with inverted flux EQ.3: CV type circuit EQ.4: CV type circuit with inverted flux R1/C1/L1/R 2/C2 Parameters (Resistances, inductances, capacities) for the different circuits. P2LCID Load curve ID describing behavior of P2(t) function of time for CV type circuit. i(t) R2 P(t) Meshed Part C1 R1 L1 Figure 5-1. Windkessel Circuit Remarks: 1. Figure 5-1 shows a Windkessel circuit and Figure 5-2 a CV circuit. i(t) R1 R2 P(t) Meshed Part C1 C2 R3 P2(t) Figure 5-2. CV Circuit *ICFD Purpose: This keyword will activate the adaptive mesh refinement feature. The solver will use an a-posteriori error estimator to compute a new mesh size bounded by the user to satisfy a maximum perceptual global error. Card 1 1 2 3 4 Variable MINH MAXH ERR MTH Type F F F Default none none none I 0 5 NIT I 0 6 7 8 VARIABLE MINH DESCRIPTION Minimum mesh size allowed to the mesh generator. The resulting mesh will not have an element smaller than MINH even if the minimum size does not satisfy the maximum error. MAXH Maximum mesh size. ERR MTH Maximum perceptual error allowed in the whole domain. Specify if the mesh size is computed based on function error or gradient error. EQ.0: Function error. EQ.1: Gradient error. NIT Number of iterations before a re-meshing is forced. Default forces a re-meshing at every timestep. *ICFD_CONTROL_ADAPT_SIZE Purpose: This keyword controls the re-meshing of elements taking into account the element quality and distortion in contrast to the default algorithm which only checks for inverted elements. Card 1 1 2 3 4 5 6 7 8 Variable ASIZE NIT Type Default I 0 I none VARIABLE ASIZE DESCRIPTION EQ.0: only re-mesh in cases where elements invert. EQ.1: re-mesh if elements invert or if element quality deterio- rates. NIT Number of iterations before a re-meshing is forced. If a negative integer is entered, then a load curve function of time will be used to define NIT. *ICFD Purpose: This keyword allows to pick between the different coupling methods for conjugate heat transfer applications Card 1 1 2 3 4 5 6 7 8 Variable CTYPE Type Default I 0 VARIABLE DESCRIPTION CTYPE Indicates the thermal coupling type. EQ.0: Robust and accurate monolithic coupling where the temperature field are solved simultaneously between the fluid and the structure. EQ.1: Weak thermal coupling. The fluid passes the heat flux to the solid at the fluid-structure interface and the solid re- turns the temperature which is applied as a Dirichlet condi- tion. Remarks: 1. The keyword ICFD_BOUNDARY_CONJ_HEAT is ignored if CTYPE = 1 but the keyword ICFD_BOUNDARY_FSI is needed in all thermal coupling cases. *ICFD_CONTROL_DEM_COUPLING Purpose: This keyword is needed to activate coupling between the ICFD and DEM solvers. 5 6 7 8 Card 1 1 Variable CTYPE Type Default I 0 2 BT F 3 DT F 4 SF F 0. 1E+28 1. VARIABLE DESCRIPTION CTYPE Indicates the coupling direction to the solver. EQ.0: two-way coupling between the fluid and the solid particles. EQ.1: one-way coupling: The DEM particles transfer their location to the fluid solver. EQ.2: one-way coupling: the DEM particles The fluid solver transfers forces to BT DT SF Birth time for the DEM coupling. Death time for the DEM coupling. Scale force which can be applied on the force by to the DEM particles. *ICFD Purpose: This keyword modifies default values for the fluid-structure interaction coupling algorithm. 4 5 6 7 8 IDC LDICSF XPROJ Card 1 1 Variable OWC Type Default I 0 2 BT F 0 3 DT F F I 0 I 0 1E+28 0.25 VARIABLE DESCRIPTION OWC Indicates the coupling direction to the solver. EQ.0: two-way coupling: Loads and displacements are transferred across the FSI interface and the full non-linear problem is solved. EQ.1: one-way coupling: The solid mechanics solver transfers displacements to the fluid solver. EQ.2: one-way coupling: The fluid solver transfers stresses to the solid mechanics solver. BT DT Birth time for the FSI coupling. Before BT the fluid solver will not pass any loads to the structure but it will receive displacements from the solid mechanics solver. Death time for the FSI coupling. After DT the fluid solver will not transfer any loads to the solid mechanics solver but the fluid will continue to deform with the solid. IDC Interaction detection coefficient. See Remark 1. LCIDSF Optional load curve ID to apply a scaling factor on the forces transferred to the solid : GT.0: Load curve ID function of iterations LT.0: Load curve ID function of time Fluid Nodes Solid Nodes Figure 5-3. Geometry of FSI contact. DESCRIPTION Projection of the nodes of the CFD domain that are at the FSI interface onto the structural mesh. EQ.0: No projection EQ.1: Projection VARIABLE XPROJ Remarks: 1. One of the criteria to automatically detect the fluid and solid surfaces that will interact in FSI problems is the distance 𝑑 between a fluid (solid) node and a solid (fluid) element respectively: 𝑑 ≤ IDC × min (ℎ, 𝐻) where ℎ is the size of the fluid mesh, 𝐻 the size of the solid mechanics mesh, and IDC a detection coefficient criteria with IDC = 0.25 by default. In the majority of cases, this default value is sufficient to ensure FSI interaction. However, it can happen in special cases that the fluid and solid geometries have curvatures that differ too much (example: pipe flows in conjugate heat transfer applications). In such cases, a bigger IDC value may be needed. This flag should be handled with care. 2. XPROJ = 1 is recommended for cases with rotation. *ICFD Purpose: This keyword allows choosing between the different types of CFD analyses (transient or steady state). Card 1 1 2 3 4 5 6 7 8 Variable ATYPE MTYPE Type Default I 0 I 0 VARIABLE DESCRIPTION ATYPE Analysis type : EQ. -1: Turns off the ICFD solver after initial keyword reading. EQ.0: Transient analysis (Default) MTYPE Solving Method type : EQ.0: Fractional Step Method EQ.1: Monolithic solve EQ.2: Potential flow solve (Steady state only) *ICFD_CONTROL_IMPOSED_MOVE Purpose: This keyword allows the user to impose a velocity on specific ICFD parts or on the whole volume mesh. Global translation, global rotation and local rotation components can be defined and combined. This can be used in order to save calculation time in certain applications such as sloshing where the modeling of the whole fluid box and the solving of the consequent FSI problem is not necessarily needed. Card 1 1 2 3 4 5 6 7 8 Variable PID LCVX LCVY LCVZ VADT Type I I I I Default none none none none I 0 Optional Card. Rotational velocity components using Euler angles . Card 2 1 2 3 4 5 6 7 8 Variable ALPHAL BETAL GAMMAL ALPHAG BETAG GAMMAG VADR Type I I I I I I Default none none none none none none I 0 Optional Card. Local reference frame definition if ALPHAL, BETAL or GAMMAL used. Card 3 1 Variable PTID Type Default I 0 2 X1 F 1. 3 Y1 F 0. 4 Z1 F 0. 5 X2 F 0. 6 Y2 F 1. 7 Z2 F 0. VARIABLE PID DESCRIPTION PID. This can be any part ID referenced in *ICFD_PART or *ICFD_PART_VOL. If PID = 0, then the whole volume mesh will be used. LCVX, LCVY, LCVZ LCID for the velocity in the three global directions (𝑥, 𝑦, 𝑧). VADT Velocity/Displacements components flag for translation EQ.0: Prescribe Velocity EQ.1: Prescribe Displacements ALPHAL, BETAL, GAMMAL LCID for the three Euler angle rotational velocities in the local reference frame . ALPHAG, BETAG, GAMMAG LCID for the three Euler angle rotational velocities in the global reference frame . VADR Velocity/Displacements components flag for rotation EQ.0: Prescribe Velocity EQ.1: Prescribe Displacements Point ID for the origin of the local reference frame. If not defined, the barycenter of the volume mesh will be used. Three components of the local reference X1 axis. If not defined, the global 𝑥 axis will be used. Three components of the local reference X2 axis. If not defined, the global 𝑦 axis will be used. PTID X1, Y1, Z1 X2, Y2, Z2 Remarks: Figure 5-4. A rotation represented by Euler angles (𝛼, 𝛽, 𝛾) using 𝐙(𝛼)𝐗(𝛽)𝐙(𝛾) intrinsic rotations. 1. Rotations. Any target orientation can be reached starting from a known reference orientation using a specific sequence of intrinsic rotations whose magnitudes are the Euler angles (𝛼, 𝛽, 𝛾). Equivalently, any rotation matrix R can be decomposed as a product of three elemental rotation matrices. For instance: 𝐑 = 𝐗(𝛼)𝐘(𝛽)𝐙(𝛾) However, different definition of the elemental rotation matrices (𝑥, 𝑦, 𝑧) and their multiplication order can be adopted. The ICFD solver uses the following approach and rotation matrix: 𝐙(𝛼)𝐗(𝛽)𝐙(𝛾) = ⎡ ⎢ ⎢ ⎢ ⎢ ⎣ 𝑐𝛼𝑐γ − 𝑐𝛽𝑠𝛼𝑠𝛾 −𝑐𝛽𝑐𝛾𝑠𝛼 − 𝑐𝛼𝑠𝛾 𝑐γ𝑠𝛼 + 𝑐𝛼𝑐𝛽𝑠𝛾 𝑐𝛼𝑐𝛽𝑐𝛾 − 𝑠𝛼𝑠𝛾 −𝑐𝛼𝑠𝛽 𝑠𝛽𝑠𝛾 𝑐𝛾𝑠𝛽 𝑠𝛼𝑠𝛽 ⎤ ⎥ ⎥ ⎥ ⎥ 𝑐𝛽 ⎦ where 𝑿(𝛼), 𝒀 (𝛽), and 𝒁(𝛾) are the matrices representing the elemental rotations about the axes (𝑥, 𝑦, 𝑧), 𝑠𝛼 = sin(𝛼), and 𝑐𝛽 = cos(𝛽). 2. Local Coordinate Systems. It is possible to have the ICFD parts or ICFD_- PART_VOLs rotate around the global reference frame but also to define and use a local reference frame by defining its point of origin and two of its vectors 𝐯1 = (X1, Y1, Z1) and 𝐯2 = (X2, Y2, Z2). The third vector is, then, in the direction of 𝐯1 × 𝐯2. See Figure 5-4. *ICFD Purpose: This keyword resets the body load in the ICFD solver to zero, while leaving the body load unchanged for the solid mechanics solver. It is useful in problems where the gravity acceleration may be neglected for the fluid problem, but not for the solid mechanics problem. Card 1 1 2 3 4 5 6 7 8 Variable ABL Type Default I 1 VARIABLE ABL DESCRIPTION EQ.0: the body load provided in *LOAD_BODY is reset to zero only for the fluid analysis. *ICFD_CONTROL_MESH Purpose: This keyword modifies default values for the automatic volume mesh generation. Card 1 1 2 3 4 5 6 7 8 Variable MGSF MSTRAT 2DSTRUC NRMSH Type F Default 1.41 I 0 I 0 I 0 VARIABLE MGSF DESCRIPTION Mesh Growth Scale Factor : Specifies the maximum mesh size that the volume mesher is allowed to use when generating the volume mesh based on the mesh surface element sizes defined in *MESH_- SURFACE_ELEMENT. MSTRAT Mesh generation strategy : EQ.0: Mesh generation based on Delaunay criteria EQ.1: Mesh generation based on octree 2DSTRUC Flag to decide between a unstructured mesh generation strategy in 2D or a structured mesh strategy : EQ.0: Structured mesh EQ.1: Unstructured mesh NRMSH Flag to turn off any remeshing : EQ.0: Remeshing possible EQ.1: Remeshing impossible Remarks: 1. For MGSF, values between 1 and 2 are allowed. Values closer to 1 will result in a finer volume mesh (1 means the volume mesh is not allowed to be coarser than the element size from the closest surface meshes) and values closer to 2 will result in a coarser volume mesh (2 means the volume can use elements as much as twice as coarse as those from the closest surface mesh). MGSF has a fixed value of 1 in 2D. 2. If the user knows in advance that no remeshing will occur during the analysis, then setting NRMSH to 1may be useful as it will free space used to back up the mesh and consequently lower memory consumption. 3. The Default Mesh generation strategy (based on Delaunay criteria) yields a linear interpolation of the mesh size between two surfaces facing each other whereas the octree based generation strategy allows for elements’ sizes to remain close to the element surface mesh size over a longer distance. This can be useful in configura- tions where two surface meshes facing each other have very distinct sizes in order to create a smoother transition. *ICFD_CONTROL_MESH_MOV Purpose: With this keyword the user can choose the type of algorithm for mesh movement. Card 1 1 2 3 4 5 6 7 8 Variable MMSH LIM_ITER RELTOL Type Default I 2 I F 100 1.0e-3 VARIABLE MMSH DESCRIPTION Mesh motion selector: EQ.-1: Completely shuts off any mesh movement. EQ.1: mesh moves based on the distance to moving walls. EQ.2: mesh moves by solving a linear elasticity problem using the element sizes as stiffness.(default) EQ.3: mesh uses a Laplacian smoothing with stiffness on edges and from node to opposite faces. Very robust, but costly. EQ.4: full Lagrangian: The mesh moves with the velocity of the flow. EQ.11: mesh moves using an implicit ball-vertex spring method. LIM_ITER RELTOL Maximum number of linear solver iterations for the ball-vertex linear system. Relative tolerance to use as a stopping criterion for the ball-vertex method iterative linear solver (conjugate gradient solver with diagonal scaling preconditioner). *ICFD Purpose: This keyword allows to choose between the Fractional Step Solver and the Monolithic Solver. Card 1 1 2 3 4 5 6 7 8 Variable SID Type Default I 0 VARIABLE DESCRIPTION SID Solver ID : EQ.0: Fractional Step Solver. Default. EQ.1: Monolithic Solver. *ICFD_CONTROL_OUTPUT Purpose: This keyword modifies default values for screen and file outputs related to this fluid solver only. Card 1 1 2 3 4 5 6 7 8 Variable MSGL OUTL DTOUT LSPPOUT ITOUT Type Default I 0 I 0 F 0 I 0 I 0 VARIABLE DESCRIPTION MSGL Message level. EQ.0: only time step information is output. EQ.1: first level solver information. EQ.2: full output information with details about linear algebra and convergence steps. EQ.4: full output information is also copied to the messag file. OUTL Output the fluid results in other file formats apart from d3plot. EQ.0: only d3plot output EQ.2: output a file with mesh statistics and the fluid results in OpenDX format. A directory named dx will be created in the work directory where the output files will be written. EQ.6: output a file with mesh statistics and the fluid results in VTK format readable by Paraview. A directory named vtk will be created in the work directory where the output files will be written. EQ.7: output a file with mesh statistic and the fluid results in VTU format readable by Paraview. A directory named vtk will be created in the work directory where the output files will be written. DTOUT Time interval to print the output when OUTL is different than 0. VARIABLE LSPPOUT ITOUT . DESCRIPTION EQ.1: outputs a file with the automatically created fluid volume mesh in a format compatible for LSPP. Iteration interval to print the output, including the d3plot files when the . selected steady state is *ICFD_CONTROL_OUTPUT_SUBDOM Purpose: Defines a specific zone that should be output in the format specified by the ICFD_CONTROL_OUTPUT card rather than the whole domain. Remeshing Control. First card specifies the shape of the output sub domain. Card 1 1 2 3 4 5 6 7 8 Variable SNAME Type A Default none Box Case. Card 2 for Sname = box Cards 2 1 2 3 4 5 6 7 8 Variable PMINX PMINY PMINZ PMAXX PMAXY PMAXZ Type F F F F F F Default none none none none none none Sphere Case. Card 2 for Sname = sphere Cards 3 1 2 3 4 5 6 7 8 Variable RADIUS CENTERX CENTERY CENTERZ Type F F F F Default none none none none Cylinder Case. Card 2 for Sname = cylinder Cards 4 1 2 3 4 5 6 7 8 Variable Radius PMINX PMINY PMAXZ PMAXX PMAXY PMAXZ Type F F F F F F F Default none none none none none none none VARIABLE DESCRIPTION SNAME Shape name. Possibilities include ‘box’, ‘cylinder’ and ‘sphere’ PMINX, Y, Z] X, Y, Z for the point of minimum coordinates PMAX[X, Y, Z] X, Y, Z for the point of maximum coordinates CENTER[X, Y, Z] Coordinates of the sphere center in cases where Sname is Sphere RADIUS Radius of the sphere if SNAME is sphere or of the cross section disk if SNAME is cylinder. *ICFD_CONTROL_PARTITION Purpose: This keyword changes the default option for the partition in MPP, thus it is only valid in MPP. Card 1 1 2 3 4 5 6 7 8 Variable PTECH Type Default I 1 VARIABLE DESCRIPTION PTECH Indicates the type of partition. EQ.1: the library Metis is used. EQ.2: partition along the axis with higher aspect ratio. EQ.3: partition along X axis. EQ.4: partition along Y axis. EQ.5: partition along Z axis. Purpose: This keyword modifies the porous media solve. *ICFD Card 1 1 2 3 4 5 6 7 8 Variable PMSTYPE Type Default I 0 VARIABLE DESCRIPTION PMSTYPE Indicates the porous media solve type. EQ.0: Anisotropic Generalized Navier-Stokes model for porous media using Fractional step method. EQ.1: Anisotropic Darcy-Forcheimer model using a Monolithic approach for the solve. This method is better suited for very low Reynolds flows through porous media (Frequent- ly encountered in Resin Transfer Molding (RTM) applica- tions). Remarks: 1. When using the Anisotropic Darcy-Forcheimer model, the convective term in the Navier Stokes formulation is neglected. *ICFD_CONTROL_STEADY Purpose: This keyword allows to specify convergence options for the steady state solver. Card 1 Variable 1 ITS 2 3 4 5 6 7 8 TOL1 TOL2 TOL3 REL1 REL2 UREL ORDER Type I F F F F F Default 1e6 1.e-3 1.e-3 1.e-3 0.3 0.7 F 1. I 0 VARIABLE ITS TOL1/2/3 REL1/2 UREL DESCRIPTION Maximum number of iterations to reach convergence. Tolerance limits for the momentum pressure and temperature equations respectfully. Relaxation parameters for the velocity and pressure respectfully. Decreasing those values may add stability but more iterations may be needed to reach convergence. Under relaxation parameter. Lowering this value may improve the final accuracy of the solution but more iterations may be needed to achieve convergence. ORDER Analysis order : EQ.0: Second order. More accurate but more time consuming. EQ.1: First order: More stable and faster but may be less accurate. *ICFD Purpose: This keyword enables automatic surface re-meshing. The objective of the re- meshing is to improve the mesh quality on the boundaries. It should not be used on a regular basis. Card 1 1 2 3 4 5 6 7 8 Variable RSRF SADAPT Type Default I 0 I 0 VARIABLE DESCRIPTION RSRF Indicates whether or not to perform a surface re-meshing. EQ.0: no re-meshing is applied. EQ.1: Laplacian smoothing surface remeshing EQ.2: Curvature preserving surface remeshing SADAPT Indicates whether or not to trigger adaptive surface remeshing. EQ.0: no adaptive surface re-meshing is applied. EQ.1: automatic surface remeshing when quality deteriorates (3D only). . *ICFD_CONTROL_TAVERAGE Purpose: This keyword controls the restarting time for computing the time average values. By default, there is no restarting and the average quantities are given starting from 𝑡 = 0. This keyword can be useful in turbulent problems that admit a steady state. 2 3 4 5 6 7 8 Card 1 Variable 1 DT Type F Default none VARIABLE DESCRIPTION DT Over each DT time interval, the average quantities are reset. *ICFD Purpose: This keyword is used to change the defaults related to time parameters in the fluid problem. Card 1 1 Variable TTM Type F Default 1028 2 DT F 0 3 4 5 6 7 8 CFL LCIDSF DTMIN DTMAX DTINIT TDEATH F 1 I F F F F none none none None 1E28 VARIABLE DESCRIPTION TTM DT CFL LCIDSF DTMIN DTMAX DTINIT TDEATH Total time of simulation for the fluid problem. Time step for the fluid problem. If different from zero, the time step will be set constant and equal to this value. If DT = 0, then the time step is automatically computed based on the CFL condition. CFL number for DT = 0. In general, CFL specifies a scale factor that is applied to the time step. When DT = 0, the time step is set to the maximum value satisfying the CFL condition, in which case this scale factor is equal to the CFL number. Load Curve ID specifying the CFL number when DT = 0 as a function of time, and more generally LCIDSF specifies the time step scale factor as the function of time. Minimum time step. When an automatic time step is used and DTMIN is defined, the time step cannot drop below DTMIN. Maximum time step. When an automatic time step is used and DTMAX is defined, the time step cannot increase beyond DTMAX. Initial time step. If not defined, the solver will automatically determine an initial timestep based on the flow velocity or dimensions of the problem in cases where there is no inflow. Death time for the Navier Stokes solve. After TDEATH, the velocity and pressure will no longer be updated. But the temperature and other similar quantities still can. *ICFD_CONTROL_TRANSIENT Purpose: This keyword allows to specify different integration scheme options for the transient solver. Card 1 1 2 3 4 5 6 7 8 Variable TORD FSORD Type Default I 0 I 0 VARIABLE DESCRIPTION TORD Time integration order : EQ.0: Second order. EQ.1: First order. FSORD Fractional step integration order : EQ.0: Second order. EQ.1: First order. *ICFD Purpose: This keyword enables the user to modify the default values for the turbulence model. Card 1 1 2 3 Variable TMOD SUBMOD WLAW Type Default I 0 I 1 Optional card if TMOD = 1. Card 2 1 2 Variable Ce1 Ce2 Type F F I 1 3 𝜎𝑒 F 4 KS F 0. 4 𝜎𝑘 F 5 CS F 0. 5 𝐶𝜇 F 6 7 8 LCIDS1 LCID2 I I none none 6 7 8 𝐶𝑐𝑢𝑡 F Default 1.44 1.92 1.3 1.0 0.09 -1. Optional card TMOD = 2 or TMOD = 3. 2 3 4 5 6 7 8 Card 2 Variable 1 Cs Type F Default 0.18 Card 2 Variable Type 1 𝛾 F 2 𝛽01 F Default 1.44 0.072 Optional card if TMOD = 4. Card 3 Variable 1 𝑎1 Type F 2 𝛽02 F Default 0.31 0.0828 Optional card if TMOD = 5. Card 2 1 Variable 𝐶𝑏1 2 𝐶𝑏1 Type F F 3 𝜎𝜔1 F 2 3 𝜎𝜔2 F 2 3 𝜎𝜈 F *ICFD_CONTROL_TURBULENCE 7 8 5 ∗ 𝛽0 F 6 𝐶𝑐𝑢𝑡 F 0.09 -1. 6 7 8 5 𝐶𝑙 F 0.875 5 6 7 8 𝐶𝑤1 𝐶𝑤2 4 𝜎𝑘1 F 2 4 𝜎𝑘2 F 2 4 𝐶𝑣1 F F F Default 0.1355 0.622 0.66 7.2 0.3 2.0 VARIABLE DESCRIPTION TMOD Indicates what turbulence model will be used. EQ.0: Turbulence model based on a variational multiscale approach is used by default. EQ.1: RANS 𝑘 - 𝜀 approach. EQ.2: LES Smagorinsky sub-grid scale model. EQ.3: LES Wall adapting local eddy-viscosity (WALE) model. EQ.4: RANS 𝑘 - 𝑤 approach. EQ.5: RANS Spalart Allmaras approach. SUBMOD Turbulence sub-model. If TMOD = 1 : EQ.1: EQ.2: Standard model Realizable model If TMOD = 4 : EQ.1: EQ.2: EQ.3: Standard Wilcox 98 model Standard Wilcox 06 model SST Menter 2003 WLAW Law of the wall ID is RANS turbulence model selected : EQ.1: Standard classic law of the wall. EQ.2: Standard Launder and Spalding law of the wall. EQ.4: Non equilibrium Launder and Spalding law of the wall. EQ.5: Automatic classic law of the wall. Roughness physical height and Roughness constant. Only used if RANS turbulence model selected. Load curve describing user defined source term in turbulent kinetic energy equation function of time. See *DEFINE_CURVE, *DE- FINE_CURVE_FUNCTION, or *DEFINE_FUNCTION. If a DE- FINE_FUNCTION is used, the following parameters are allowed: 𝑓 (𝑥, 𝑦, 𝑧, 𝑣𝑥, 𝑣𝑦, 𝑣𝑧, 𝑡𝑒𝑚𝑝, 𝑝𝑟𝑒𝑠, 𝑡𝑖𝑚𝑒, 𝑘, 𝑒, 𝑚𝑢𝑡). KS/CS LCIDS1 LCIDS2 *ICFD_CONTROL_TURBULENCE DESCRIPTION Load curve describing user defined source term in turbulent dissipation equation function of time. See *DEFINE_CURVE, *DE- FINE_CURVE_FUNCTION, or *DEFINE_FUNCTION. If a DE- FINE_FUNCTION is used, the following parameters are allowed: 𝑓 (𝑥, 𝑦, 𝑧, 𝑣𝑥, 𝑣𝑦, 𝑣𝑧, 𝑡𝑒𝑚𝑝, 𝑝𝑟𝑒𝑠, 𝑡𝑖𝑚𝑒, 𝑘, 𝑒, 𝑚𝑢𝑡). Ce1, Ce2, 𝜎𝑒, 𝜎𝑘, 𝐶𝜇, 𝐶𝑐𝑢𝑡 𝑘 - 𝜀 model constants Cs Smagorinsky constant if TMOD = 2 or WALE constant if TMOD = 3 𝑘 -𝜔 model constants Spalart-Allmaras constants 𝛾, 𝛽01, 𝜎𝜔1, 𝜎𝑘1, 𝛽0 ∗, 𝑎1, 𝛽02, 𝜎𝜔2, 𝜎𝑘2, 𝐶𝑙, 𝐶𝑐𝑢𝑡 𝐶𝑏1,𝐶𝑏2,𝜎𝜈, 𝐶𝑣1, 𝐶𝑤1𝐶𝑤2 Remarks: 1. For the Standard 𝑘 - 𝜀 model, the following two equations are solved for the turbulent kinetic energy and the turbulent dissipation respectively 𝑘 and 𝜀 : 𝜕𝑘 𝜕𝑡 + 𝜕(𝑘𝑢𝑖) 𝜕𝑥𝑖 = 𝜕 𝜕𝑥𝑗 [( + 𝜇𝑡 𝜌 𝜎𝑘 ) 𝜕𝑘 𝜕𝑥𝑗 ] + 𝑃𝑘 + 𝑃𝑏 − 𝜖 + 𝑆𝑘 𝜕𝜖 𝜕𝑡 + 𝜕(𝜖𝑢𝑖) 𝜕𝑥𝑖 = 𝜕 𝜕𝑥𝑗 [( + 𝜇𝑡 𝜌 𝜎𝜖 ) 𝜕𝜖 𝜕𝑥𝑗 ] + 𝐶1𝜖 𝑃𝑘 − 𝐶2𝜀 𝜖2 + 𝑆𝑒 With 𝑃𝑘 the 𝑘 production term, 𝑃𝑏 the production term due to buoyancy and 𝑆𝑘, 𝑆𝑒 are the user defined source terms. 𝑃𝑘 and 𝑃𝑏 are expressed as : 𝑃𝑘 = 𝜇𝑡 𝑆2 𝑃𝑏 = 𝛽𝜇𝑡 𝜌𝑃𝑟𝑡 𝑔𝑖 𝜕𝑇 𝜕𝑥𝑖 With 𝑆 the modulus of the mean rate of strain tensor (𝑆2 = 2𝑆𝑖𝑗𝑆𝑖𝑗), 𝛽 the coefficient of thermal expansion, and 𝑃𝑟𝑡 the turbulent Prandtl number. The turbulent viscosi- ty is then expressed as: 𝜇𝑡 = 𝜌𝐶𝜇 𝑘2 For the realizable 𝑘 - 𝜀 model, the equation for the turbulent kinetic energy does not change, but the equation for the turbulent dissipation is now expressed as: 𝜕𝜖 𝜕𝑡 + 𝜕(𝜖𝑢𝑖) 𝜕𝑥𝑖 = 𝜕 𝜕𝑥𝑗 [( + 𝜇𝑡 𝜌 𝜎𝜖 ) 𝜕𝜖 𝜕𝑥𝑗 ] + 𝐶1𝑆𝜖 − 𝐶2𝜀 𝜖2 𝑘 + √ 𝜌 𝜖 − 𝜖 + 𝑆𝑒 With 𝐶1 = 𝑚𝑎𝑥[0.43, 𝜂+5], 𝜂 = 𝑆 𝑘 𝜖. Furthermore, while the turbulent viscosity is still expressed the same way, 𝐶𝜇 is no longer a constant: 𝐶𝜇 = 𝐴0 + 𝐴𝑠𝑘 𝑈∗ 𝑈∗ = √Ω𝑖𝑗Ω𝑖𝑗 + 𝑆𝑖𝑗𝑆𝑖𝑗 𝐴0 = 4.04 𝐴𝑠 = √6𝑐𝑜𝑠 (1 3 𝑐𝑜𝑠−1 (√6 𝑆𝑖𝑗𝑆𝑗𝑘𝑆𝑘𝑖 (𝑆𝑖𝑗𝑆𝑖𝑗)3/2)) It can be noted that in this case, the constant value 𝐶𝜇 that can be input by the user serves as the limit values that 𝐶𝜇 can take. By default 𝐶𝜇 = 0.09 so: 0.0009 < 𝐶𝜇 < 0.09 2. For the Standard Wilcox 06 𝑘 -𝜔 model, the following two equations are solved for the turbulent kinetic energy and the specific turbulent dissipation rate respectively 𝑘 and 𝜔 : 𝜕𝑘 𝜕𝑡 + 𝜕(𝑘𝑢𝑖) 𝜕𝑥𝑖 = 𝜕 𝜕𝑥𝑗 [( + 𝜇𝑡 𝜌 𝜎𝑘1 ) 𝜕𝑘 𝜕𝑥𝑗 ] + 𝑃𝑘 − 𝛽∗𝑘𝜔 + 𝑆𝑘 𝜕𝑤 𝜕𝑡 + 𝜕(𝑤𝑢𝑖) 𝜕𝑥𝑖 = 𝜕 𝜕𝑥𝑗 [( + 𝜇𝑡 𝜌 𝜎𝑤1 ) 𝜕𝜖 𝜕𝑥𝑗 ] + 𝛾 𝑃𝑘 − 𝛽𝜔2 + 𝜎𝑑𝑋𝑘𝜔2 + 𝑆𝜔 With 𝑃𝑘 the 𝑘 production term and 𝑆𝑘, 𝑆𝜔 are the user defined source terms. 𝑃𝑘, 𝛽∗ and 𝛽 are expressed as: 𝑃𝑘 = 𝜇𝑡 𝑆2 𝛽∗ = 𝛽0 ∗𝑓𝛽∗ 𝛽 = 𝛽01𝑓𝛽 𝑓𝛽 = 1 + 85𝑋𝜔 1 + 100𝑋𝜔 𝑓𝛽∗ = 1. 𝜎𝑑 = { 0. 𝑋𝑘 ≤ 0. 1/8 𝑋𝑘 > 0. 𝑋𝑘 = 𝜔3 𝜕𝑘 𝜕𝑥𝑗 𝜕𝜔 𝜕𝑥𝑗 𝑋𝜔 = ∣ Ω𝑖𝑗Ω𝑗𝑘S𝑘𝑖 ∗𝜔)3 ∣ (𝛽0 The turbulent viscosity is then: 𝜇𝑡 = 𝜌 𝑚𝑎𝑥 ⎡ 𝜔, 𝐶𝑙√ ⎢ ⎣ 2𝑆𝑖𝑗𝑆𝑖𝑗 ∗ 𝛽0 ⎤ ⎥ ⎦ For the Standard Wilcox 98 model, the following terms are modified: 𝑓𝛽 = 1 + 70𝑋𝜔 1 + 80𝑋𝜔 𝑓𝛽∗ = {{⎧ {{⎨ ⎩ 1 𝑋𝑘 ≤ 0. 2 𝑋𝑘 > 0. 1 + 680 𝑋𝑘 1 + 400 𝑋𝑘 𝜎𝑑 = 0. The turbulent viscosity is then: 𝜇𝑡 = 𝜌 For the Menter SST 2003 model, the following equations are solved: 𝜕𝑘 𝜕𝑡 + 𝜕(𝑘𝑢𝑖) 𝜕𝑥𝑖 = 𝜕 𝜕𝑥𝑗 [( + 𝜇𝑡 𝜌 𝜎𝑘 ) 𝜕𝑘 𝜕𝑥𝑗 ] + 𝑃𝑘 − 𝛽0 ∗𝑘𝜔 + 𝑆𝑘 𝜕𝑤 𝜕𝑡 + 𝜕(𝑤𝑢𝑖) 𝜕𝑥𝑖 = 𝜕 𝜕𝑥𝑗 [( + 𝜇𝑡 𝜌 𝜎𝑤 ) 𝜕𝜖 𝜕𝑥𝑗 ] + 𝜇𝑡 𝑃𝑘 − 𝛽𝜔2 + 2(1 − 𝐹1) 𝜎𝑤2𝑋𝑘𝜔2 + 𝑆𝜔 Each of the constants, 𝛾, 𝛽, 𝜎𝑘, 𝜎𝑤 are now computed by a blend via: Where the blending function 𝐹1 is defined by: 𝛼 = 𝛼1𝐹1 + 𝛼2(1 − 𝐹1) 𝐹1 = tanh ⟨ ⎡𝑚𝑖𝑛 ⎢ ⎣ ⎜⎜⎛𝑚𝑎𝑥 ⎝ ⎜⎜⎛ √𝑘 ∗𝜔𝑦 𝛽0 ⎝ , 500𝜈 ⎟⎟⎞ , 𝑦2𝜔 ⎠ 4𝜌𝜎𝑤2𝑘 𝐶𝐷 𝑦2 ⎤ ⎥ ⎦ ⎟⎟⎞ ⎠ ⟩ With 𝑦 the distance to the nearest wall and: 𝐶𝐷 = 𝑚𝑎𝑥(2𝜌𝜎𝜔2𝑋𝑘𝜔2, 10−10) The turbulent viscosity is then: 𝜇𝑡 = 𝜌 𝑎1𝑘 𝑚𝑎𝑥(𝑎1𝜔, 𝑆 𝐹2) With: 𝐹2 = 𝑡𝑎𝑛ℎ 𝑚𝑎𝑥 ⎜⎜⎛ 2√𝑘 ∗𝜔𝑦 𝛽0 ⎝ , 500𝜈 ⎟⎟⎞ 𝑦2𝜔 ⎠ ⎡ ⎜⎜⎜⎜⎛ ⎢⎢ ⎝ ⎣ ⎟⎟⎟⎟⎞ ⎠ ⎤ ⎥⎥ ⎦ 3. It is possible to activate a limiter on the production term 𝑃𝑘. If 𝐶𝑐𝑢𝑡 ≥ 0., then : 𝑃𝑘 = 𝑚𝑖𝑛(𝑃𝑘, 𝐶𝑐𝑢𝑡𝜀) if TMOD = 1, 𝑃𝑘 = 𝑚𝑖𝑛(𝑃𝑘, 𝐶𝑐𝑢𝑡𝛽0 especially common when using the Menter SST 2003 model. ∗𝑘𝜔) if TMOD = 4. This is 4. For RANS models, the following laws of the wall are available : a) STANDARD CLASSIC : 𝑈+ = ln (𝐸 𝑌+) If 𝑌+ > 11.225, 𝑈+ = 𝑌+ otherwise 𝜌𝑦𝑈𝜏 𝑌+ = 𝑈+ = 𝑈𝜏 𝑈𝜏 = √ 𝜏𝑤 This is the default for TMOD = 1 b) STANDARD LAUNDER and SPALDING : 𝑈∗ = ln(𝐸 𝑌∗) If 𝑌∗ > 11.225, 𝑈∗ = 𝑌∗ otherwise 𝑌∗ = 𝜌𝐶𝜇 1/4𝑘1/2𝑦 𝑈∗ = 𝑈𝐶𝜇 1/4𝑘1/2 𝑈𝜏 𝑈𝜏 = √ 𝜏𝑤 c) The NON EQUILIBRUM laws of the wall modify the expression of the ve- locity at the wall making it sensitive to the pressure gradient : 𝑈 = 𝑈 − ⎡ 𝑦𝑣 𝑑𝑃 ⎢ 𝑑𝑥 ⎣ 𝜌𝜅√𝑘 𝑙𝑛 ( 𝑦𝑣 ) + 𝑦 − 𝑦𝑣 𝜌𝜅√𝑘 + 𝑦𝑣 ⎤ ⎥ 𝜇 ⎦ With: 𝑦𝑣 = 11.225 𝑦∗ 𝑦 This law is recommended with TMOD = 1 and in cases of complex flows involving separation, reattachment and recirculation. d) The automatic wall law attempts to blend the viscous and log layers to bet- ter account for the transition zone. In the buffer region, we have : 𝑈+ = 𝑈𝜏 𝑈𝜏 = √ √√ ⎷ 𝑦+)4 + ( ( 𝜅 ln (𝐸𝑦+) )4 This is the recommended approach for TMOD = 4. 5. The LES Smagorinsky turbulence model uses the Van Driest damping function close to the wall : 𝑓𝑣 = 1 − 𝑒 − 𝑦+ 𝐴+ 6. When a RANS turbulence model is selected, it is possible to define extra parame- ters to account for the rugosity effects. In such cases, an extra term will be added to the logarithmic part of the different laws of the wall : 𝑈+ = ln(𝐸 𝑌+) − Δ𝐵 If we introduce the non-dimensional roughness height 𝐾+ = 1/4𝑘1/2 𝜌𝐾𝑠𝐶𝜇 , we have: Δ𝐵 = 0 𝑓𝑜𝑟 𝐾+ ≤ 2.25 Δ𝐵 = 𝑙𝑛 [ 𝐾+ − 2.25 87.75 + 𝐶𝑠𝐾+] × 𝑠𝑖𝑛(0.4258(ln 𝐾+ − 0.811)) 𝑓𝑜𝑟 2.25 < 𝐾+ ≤ 90.0 Δ𝐵 = 𝑙𝑛(1 + 𝐶𝑠𝐾+) 𝑓𝑜𝑟 90. < 𝐾+ *ICFD_CONTROL_TURB_SYNTHESIS Purpose: This keyword enables the user impose a divergence-free turbulent field on inlets. Card must be used jointly with VAD = 4 of keyword *ICFD_BOUNDARY_PRESCRIBED_- VEL. Card 1 1 Variable PID Type Default I 0 2 IU F 3 IV F 4 IW F 5 LS F 10-3 10-3 10-3 ℎ𝑚𝑖𝑛 6 7 8 VARIABLE DESCRIPTION PID Part ID of the surface with the turbulent velocity inlet condition. IU, IV, IW Intensity of field fluctuations over 𝑥, 𝑦, and 𝑧 directions, IU = 𝑢′ 𝑢avg . LS Integral length scale of turbulence Remarks: 1. If this card is not defined but a turbulent field inlet has been activated. See VAD = 4 of *ICFD_BOUNDARY_PRESCRIBED_VEL, the default parameters will be used. *ICFD Purpose: This keyword enables the computation of time average variables at given time intervals. 2 3 4 5 6 7 8 DESCRIPTION Over each DT time interval, an average of the different fluid variables will be calculated and then reset when moving to the next DT interval. Card 1 Variable 1 DT Type F Default none VARIABLE DT Remarks: 1. The file name for this database is icfdavg.*.dat with the different averaged variable values copied in a ASCII format. *ICFD_DATABASE_DRAG_{OPTION} Available options include VOL Purpose: This keyword enables the computation of drag forces over given surface parts of the model. If multiple keywords are given, the forces over the PID surfaces are given in separate files and are also added and output in a separate file. For the VOL option, drag calculation can also be applied on a volume defined by ICFD_PART_VOL. This is mostly useful in porous media applications to output the pressure drag of the porous media domain. Surface Drag Cards. Include one card for each surface on which drag is applied. This input ends at the next keyword (“*”) card. Card 1 1 2 3 4 5 6 7 8 Variable PID CPID DTOUT PEROUT DIVI ELOUT SSOUT Type I I F Default none none 0. I 0 I 10 I 0 I 0 VARIABLE DESCRIPTION PID CPID DTOUT PEROUT DIVI Part ID of the surface where the drag force will be computed. Center point ID used for the calculation of the force’s moment. By default the reference frame center is used is 𝟎 = (0, 0, 0). Time interval to print the output. If DTOUT is equal to 0.0, then the ICFD timestep will be used. Outputs the contribution of the different elements on the total drag in fractions of the total drag in the d3plots. Number of drag divisions for PEROUT. Default is 10 which means the contributions will be grouped in 10 deciles. ELOUT Outputs the drag value of each element in the d3plots. SSOUT Outputs the pressure loads caused by the fluid on each solid segment set in keyword format. FSI needs to be activated. *ICFD 1. The file name for this database is icfdragi for instantaneous drag and icfdraga for the drag computed using average values of pressure and velocities. 2. The output contains: a) “Fpx” , “Fpy”, and “Fpz” refer to the three components of the pressure drag force where 𝑃 is the pressure and 𝐴 the surface area. 𝐅𝑝 = ∫ 𝑃𝑑𝑨, b) “Fvx”, “Fxy”, and “Fvz” refer to the three components of the viscous drag force 𝐅𝑣 = ∫ 𝜇 𝜕u 𝜕y d𝑨. where 𝜕u face area. 𝜕y is the shear velocity at the wall, 𝜇 is the viscosity and 𝐴 is the sur- c) “Mpx”, “Mpy”, “Mpz”, “Mvx”, “Mvy”, and “Mvz” refer to the three compo- nents of the pressure and viscous force moments respectively. *ICFD_DATABASE_FLUX Purpose: This keyword enables the computation of the flow rate and average pressure over given parts of the model. If multiple keywords are given, separate files are output. Include as many cards as needed. This input ends at the next keyword (“*”) card. Card 1 1 2 3 4 5 6 7 8 Variable PID Type I Default none VARIABLE DESCRIPTION PID Part ID of the surface where the flow rates will be computed. Remarks: 1. The file name for this database is icfd_flux.dat. 2. The flux database contains the flow rate through a section, called “output flux”, the average pressure, called “Pre-avg”, 𝛷 = ∑(𝐕𝑖 ⋅ 𝐧𝑖)𝐴𝑖 , 𝑃avg = ∑ 𝑃𝑖𝐴𝑖 ∑ 𝐴𝑖 , and the total area, called “Areatot”. *ICFD Purpose: This keyword allows the user to trigger the calculation of the Heat transfer coefficient using different methods and to control the output options. Card 1 1 2 Variable OUT HTC Type Default I 0 I 0. 3 TB F 0. 4 5 6 7 8 OUTDT F 0. VARIABLE OUT DESCRIPTION Determines if the solver should calculate the heat transfer coefficient and how to output it : EQ.0: No HTC calculation EQ.1: HTC calculated and output in LSPP as a surface variable. EQ.2: The solver will also look for FSI boundaries and output the HTC value at the solid nodes in an ASCII file called icfdhtci.dat. EQ.3: The solver will also look for FSI boundaries that are part of SEGMENT_SETS and output the HTC for those segments in an ASCII file called icfd_convseg.****.key in a format that can directly read by LS-DYNA for a subsequent pure structural thermal analysis. HTC Determines how the HTC is calculated. EQ.0: Automatically calculated by the solver based on the average temperature flowing through the pipe section . EQ.1: User imposed value . TB Value of the bulk temperature if HTC = 1. OUTDT Output frequency of the HTC in the various ASCII files. If left to 0., the solver will output the HTC at every timestep. *ICFD_DATABASE_HTC 1. The heat transfer coefficient is frequently used in thermal applications to estimate the effect of the fluid cooling and it derived from a CFD calculation. 2. The heat transfer coefficient is defined as follows: ℎ = 𝑇𝑠 − 𝑇𝑏 with 𝑞 the heat flux, 𝑇𝑠 the surface temperature and 𝑇𝑏 the so called “bulk” tem- perature. For external aerodynamic applications, this bulk temperature is often defined as a constant (ambient or far field conditions, HTC = 1). However, for internal aerodynamic application, this temperature is often defined as an average temperature flowing through the pipe section with the flow velocity being used as a weighting factor (HTC = 0). *ICFD Purpose: This keyword enables the computation of the average quantities on surface nodes defined in *ICFD_DATABASE_NODOUT. 2 3 4 5 6 7 8 Card 1 Variable Type Default 1 ON I 0 VARIABLE DESCRIPTION ON If equal to 1, the average quantities will be computed. Remarks: 1. The file name for this database is icfd_nodeavg.dat. *ICFD_DATABASE_NODOUT Purpose: This keyword enables the output of ICFD data on surface nodes. For data in the fluid volume, it is advised to use points or tracers . Output Options Card. Card 1 1 2 3 4 5 6 7 8 Variable OUTLV DTOUT Type Default I 0 F 0. Include as many cards as needed. This input ends at the next keyword (“*”) card. Card 2 1 2 3 4 5 6 7 8 Variable NID1 NID2 NID3 NID4 NID5 NID6 NID7 NID8 Type I I I I I I I I Default none none none none none none none none VARIABLE DESCRIPTION OUTLV Determines if the output file should be dumped. EQ.0: No output file is generated. EQ.1: The output file is generated. DTOUT Time interval to print the output. If DTOUT is equal to 0.0, then the ICFD timestep will be used. NID.. Node IDs. Remarks: 1. The file name for this database is icfd_nodout.dat. *ICFD Purpose: This keyword enables the computation of the average quantities on point sets using the parameters defined in *ICFD_DATABASE_POINTOUT. 2 3 4 5 6 7 8 Card 1 Variable Type Default 1 ON I 0 VARIABLE DESCRIPTION ON If equal to 1, the average quantities will be computed. Remarks: 1. The file name for this database is icfd_psavg.dat. *ICFD_DATABASE_POINTOUT Purpose: This keyword enables the output of ICFD data on points. Output Options Card. Card 1 1 2 3 Variable PSID DTOUT PSTYPE Type Default I 0 F 0. I 0 4 VX F 0. 5 VY F 0. 6 VZ F 0. 7 8 Include as many cards as needed. This input ends at the next keyword (“*”) card. 5 6 7 8 Card 2 1 Variable PID Type I 2 X F 3 Y F 4 Z F Default none none none none VARIABLE DESCRIPTION PSID Point Set ID. DTOUT Time interval to print the output. If DTOUT is equal to 0.0, then the ICFD timestep will be used. PSTYPE Point Set type : EQ.0: Fixed points. EQ.1: Tracer points using prescribed velocity. EQ.2: Tracer points using fluid velocity. EQ.3: Tracer points using mesh velocity.. VX, VY, VZ Constant velocities to be used when PSTYPE = 1 PID Point ID VARIABLE DESCRIPTION X, Y, Z Point initial coordinates Remarks: 1. The file name for this database is icfd_pointout.dat. *ICFD_DATABASE_RESIDUALS Purpose: This keyword allows the user to output the residuals of the various systems. Card 1 1 2 3 4 5 6 7 8 Variable RLVL Type Default I 0 VARIABLE DESCRIPTION RLVL Residual output level : EQ.0: No output. EQ.1: Only outputs the number of iterations needed for solving the pressure Poisson equation. EQ.2: Outputs the number of iterations for the momentum, pressure, mesh movement and temperature equations. EQ.3: Also gives the residual for each iteration during the solve of the momentum, pressure, mesh movement and tempera- ture equations. Remarks: 1. The file names for the momentum, pressure, mesh movement and temperature equations are called icfd_residuals.moms.dat, icfd_residuals.pres.dat, icfd_- residuals.mmov.dat, and icfd_residuals.temp.dat respectively. *ICFD Purpose: This keyword enables the computation of the average temperature and the heat flux over given parts of the model. If multiple keywords are given, separate files are output. Include as many cards as needed. This input ends at the next keyword (“*”) card. Card 1 1 2 3 4 5 6 7 8 Variable PID Type I Default none VARIABLE PID Remarks: DESCRIPTION Part ID of the surface where the average temperature and heat flux will be computed. 1. The file name for this database is icfd_thermal.dat. 2. Two average temperature are given in the icfd_thermal.dat file: “Temp-avg” and “Temp-sum”. The average temperature is calculated using the local node area as weighting factor, 𝑇avg = ∑ 𝑇𝑖𝐴𝑖 ∑ 𝐴𝑖 , whereas, the sum is not weighted by area 𝑇sum = ∑ 𝑇𝑖 If the mesh is regular, the two values will be of similar value. The icfd_thermal.dat output file also includes the average heat flux, the total surface area, and the aver- age heat transfer coefficients . *ICFD_DATABASE_TIMESTEP Purpose: This keyword enables the output of ICFD data regarding the ICFD timestep. Output Options Card. Card 1 1 2 3 4 5 6 7 8 Variable OUTLV Type Default I 0 VARIABLE DESCRIPTION OUTLV Determines if the output file should be dumped. EQ.0: No output file is generated. EQ.1: The output file is generated. Remarks: 1. The file name for this database is icfd_tsout.dat. 2. Outputs the run’s ICFD timestep versus the timestep calculated using the ICFD CFL condition as criteria (autotimestep). This can be useful in cases using a fixed timestep where big mesh deformations and/or big fluid velocity changes occur in order to track how that fixed timestep value compares to the reference auto- timestep. *ICFD Purpose: This keyword allows the user to have the solver calculate the uniformity index . Card 1 1 2 3 4 5 6 7 8 Variable OUT Type Default I 0 VARIABLE DESCRIPTION OUT Determines if the solver should calculate the uniformity index. EQ.0: Off. EQ.1: On. Remarks: 1. Uniformity Index. The uniformity index is a post treatment quantity which measures how uniform the flow is through a given section. It is especially useful in internal aerodynamics cases. It is expressed as : ⎡√(𝑢𝑖 − 𝑢̅)2 ⎢⎢ 𝑢̅ ⎣ with 𝐴𝑖, the local cell area, 𝐴 the total section area, 𝑢𝑖 the local velocity, 𝑢̅ the aver- age velocity through the section, and 𝑛 the number of cells. 2𝑛𝐴 ∑ 𝑖=1 𝛾 = 1 − ⎤ ⎥⎥ ⎦ 𝐴𝑖 Values close to 0 means that the flow is very unevenly distributed. This can be used to identify bends, corners or turbulent effects. Values close to 1 imply smooth or equally distributed flow through the surface. *ICFD_DEFINE_POINT Purpose: This keyword defines a point in space that could be used for multiple purposes. 5 6 7 8 Card 1 1 Variable POID Type I 2 X F 3 Y F 4 Z F Default none none none none Optional Card 2. Load curve IDS specifying velocity components of translating point Card 2 1 2 3 4 5 6 7 8 Variable LCIDX LCIDY LCIDZ Type Default I 0 I 0 I 0 Optional Card 3. Load curve IDS and rotation axis of rotating point Card 2 1 Variable LCIDW Type Default I 0 2 XT F 3 YT F 4 ZT F 5 XH F 6 YH F 7 ZH F 8 none none none none none none VARIABLE DESCRIPTION POID X/Y/Z Point ID. x, y ,z coordinates for the point. VARIABLE DESCRIPTION LCIDX/LCIDY/LCIDZ The point can be made to translate. Those are the three load curve IDs for the three translation components. LCIDW The point can also be made to rotate. This load curve specifies the angular velocity. XT/YT/ZT Rotation axis tail point coordinates. XH/YH/ZH Rotation axis head point coordinates. . *ICFD_DEFINE_NONINERTIAL Purpose: This keyword defines a non-inertial reference frame in order to avoid heavy mesh distortions and attendant remeshing associated with large-scale rotations. This is used to model, for example, spinning cylinders, wind turbines, and turbo machinery. Include as many cards as needed. This input ends at the next keyword (“*”) card. Card 1 Variable 1 W1 2 W2 3 W3 Type F F F 4 R F 5 PTID I 6 L F 7 8 LCID RELV I I 0 Default none none none none none none none VARIABLE DESCRIPTION W1, W2, W3 Rotational Velocity along the X,Y,Z axes R PTID Radius of the rotating reference frame Starting point ID for the reference frame L Length of the rotating reference frame LCID Load curve for scaling factor of w → + PTID Figure 5-5. Non Inertial Reference Frame Example VARIABLE DESCRIPTION RELV Velocities computed and displayed: EQ.0: Relative velocity, only the non-rotating components of the velocity are used and displayed. EQ.1: Absolute velocity . All the components of the velocity are used. Useful in cases where several or at least one non- inertial reference frame is combined with an inertial “clas- sical” reference frame. *ICFD_DEFINE_WAVE_DAMPING Purpose: This keyword defines a damping zone for free surface waves. Card 1 1 Variable PID 2 NID Type I F 3 L F 4 F1 F 5 F2 F Default none none 10 10 6 N I 1 7 8 LCID I none VARIABLE DESCRIPTION PID NID L F1/F2 N LCID . Point ID defining the start of the damping layer. Normal ID defined using ICFD_DEFINE_POINT and pointing to the outgoing direction of the damping layer. Length of damping layer. If no is value specified, the damping layer will have a length corresponding to five element lengths. Linear and quadratic damping factor terms. Damping term factor. Load curve ID acting as temporal scale factor on damping term. *ICFD Purpose: Simple initialization of velocity and temperature within a volume. Include as many cards as needed. This input ends at the next keyword (“*”) card. Card 1 1 Variable PID Type I 2 Vx F 3 Vy F 4 Vz F 5 T F 6 P F 7 8 Default none none none none none none VARIABLE PID DESCRIPTION Part ID for the volume elements or the surface elements where the values are initialized . PID = 0 to assign the initial condition to all nodes at once. Vx Vy Vz T P x coordinate for the velocity. y coordinate for the velocity. z coordinate for the velocity. Initial temperature. Initial Pressure. *ICFD_INITIAL_TURBULENCE Purpose: When a RANS turbulent model is selected, it is possible to modify the default initial values of the turbulent quantities using this keyword. Include as many cards as needed. This input ends at the next keyword (“*”) card. 4 5 6 7 8 Card 1 1 Variable PID Type I 2 I F 3 R F Default none none none VARIABLE DESCRIPTION Part ID for the volume elements or the surface elements where the values are initialized . PID = 0 to assign the initial condition to all nodes at once. Initial turbulent intensity. Initial turbulent viscosity to laminar viscosity ratio (𝑟 = 𝜇𝑡𝑢𝑟𝑏 𝜇 ). PID I R Remarks: 1. If no initial conditions have been assigned to a specific PID, the solver will automatically pick I = 0.05 (5%) and R = 10000. Available options include TITLE *ICFD Purpose: Specify physical properties for the fluid material. Fluid Material Card Sets: The Material Fluid Parameters Card is required. If a second card is given, it must be a Thermal Fluid Parameters Card. If the fluid thermal properties are not needed, the second card can be a blank card. In the third card, it is possible to associate the fluid material to a Non-Newtonian model and/or to a Porous media model . Material Fluid Parameters Card. Card 1 1 2 Variable MID FLG Type I Default none I 1 3 RO F 0 4 VIS F 0 5 ST F 0 6 7 8 Thermal Fluid Parameters Card. Only to be defined if the thermal problem is solved. Card 2 Variable Type Default 1 HC F 0 2 TC F 0 3 4 5 6 7 8 BETA PRT HCSFLCID TCSFLCID F 0 F I I 0.85 none none Additional fluid models. Only to be defined if the fluid is non-newtonian and/or is a porous media. Card 3 1 2 3 4 5 6 7 8 Variable NNMOID PMMOID Type I I Default none none VARIABLE DESCRIPTION MID FLG RO VIS ST HC TC BETA PRT Material ID. Flag to choose between fully incompressible, slightly compressible, or barotropic flows. EQ.0 : Vacuum (free surface problems only) EQ.1 : Fully incompressible fluid. Flow density. Dynamic viscosity. Surface tension coefficient. Heat capacity. Thermal conductivity. Thermal expansion coefficient used in the Boussinesq approxima- tion for buoyancy. Turbulent Prandlt number. Only used if K-Epsilon turbulence model selected. HCSFLCID Load curve ID for scale factor applied on HC function of time. See *DEFINE_CURVE, *DEFINE_CURVE_FUNCTION, or *DEFINE_- FUNCTION. If a DEFINE_FUNCTION is used, the following parameters are allowed: 𝑓 (𝑥, 𝑦, 𝑧, 𝑣𝑥, 𝑣𝑦, 𝑣𝑧, 𝑡𝑒𝑚𝑝, 𝑝𝑟𝑒𝑠, 𝑡𝑖𝑚𝑒). Load curve ID for scale factor applied on TC function of time. See *DEFINE_CURVE, *DEFINE_CURVE_FUNCTION, or *DEFINE_- FUNCTION. If a DEFINE_FUNCTION is used, the following parameters are allowed: 𝑓 (𝑥, 𝑦, 𝑧, 𝑣𝑥, 𝑣𝑦, 𝑣𝑧, 𝑡𝑒𝑚𝑝, 𝑝𝑟𝑒𝑠, 𝑡𝑖𝑚𝑒). Non-Newtonian model ID. This refers to a Non-Newtonian fluid model defined using *ICFD_MODEL_NONNEWT. Porous media model ID. This refers to a porous media model defined using *ICFD_MODEL_POROUS. *ICFD_MAT VARIABLE TCSFLCID NNMOID PMMOID Remarks: 1. If a K-Epsilon turbulence model is used and the heat transfer equation is solved, then the effective thermal conductivity will be determined by : 𝑘𝑒𝑓𝑓 = 𝑘 + 𝐶𝑝𝜇𝑡𝑢𝑟𝑏 𝑃𝑟𝑡𝑢𝑟𝑏 *ICFD_MODEL_NONNEWT Purpose: Specify a non-newtonian model or a viscosity law that can associated to a fluid material. Non-Newtonian Model ID and type. Card 1 1 2 3 4 5 6 7 8 Variable NNMOID NNID Type I I Default none none Non-Newtonian Fluid Parameters Card. Card 2 Variable Type 1 K F 2 N F 3 4 5 6 7 8 MUMIN LAMBDA ALPHA TALPHA F F F F Default 0.0 0.0 0.0 1.e30 0.0 0.0 VARIABLE DESCRIPTION NNMOID Non-Newtonian Model ID. NNID Non-Newtonian fluid model type : EQ.1 : Power-Law model EQ.2 : Carreau model EQ.3 : Cross model EQ.4 : Herschel-Bulkley model EQ.5 : Cross II model EQ.6 : Sutherland formula for temperature dependent viscosity EQ.7 : Power-Law for temperature dependent viscosity EQ.8 : Viscosity defined by Load Curve ID or Function ID VARIABLE DESCRIPTION K N MUMIN LAMBDA Consistency index if NNID = 1 and 4. Zero shear Viscosity if NNID = 2,3 and 5.Reference viscosity if NNID = 6 and NNID = 7. Load curve ID or function ID if NNID = 8. Measure of the deviation of the fluid from Newtonian (Power Law index) for NNID = 1,2,3,4,5,7. Not used for NNID = 6 and 8. Minimum acceptable viscosity value if NNID = 1. Infinite Shear Viscosity if NNID = 2,5.Yielding viscosity if NNID = 4.Not used if NNID = 3,6,7,8. Maximum acceptable viscosity value if NNID = 1. Time constant if NNID = 2, 3, 5. Yield Stress Threshold if NNID = 4.Sutherland constant if NNID = 6. Not used if NNID = 7,8. ALPHA Activation energy if NNID = 1, 2. Not used if NNID = 3,4,5,6,7,8. TALPHA Reference temperature if NNID = 2. Not used if NNID = 1,3,4,5,6,7,8 Remarks: 1. For the Non-Newtonian models, the viscosity is expressed as : a) POWER-LAW : 𝜇 = 𝑘𝛾̇ 𝑛−1𝑒𝛼𝑇0 𝑇⁄ 𝜇𝑚𝑖𝑛 < 𝜇 < 𝜇𝑚𝑎𝑥 With 𝑘 the consistency index, 𝑛 the power law index, 𝛼 the activation energy, 𝑇0 the initial temperature, 𝑇 the temperature at any given time 𝑡, 𝜇𝑚𝑖𝑛 the mini- mum acceptable viscosity and 𝜇𝑚𝑎𝑥 the maximum acceptable viscosity. b) CARREAU : 𝜇 = 𝜇∞ + (𝜇0 − 𝜇∞)[1 + (𝐻(𝑇)𝛾̇𝜆)2](𝑛−1) 2⁄ 𝐻(𝑇) = 𝑒𝑥𝑝 [𝛼( 𝑇 − 𝑇0 − 𝑇𝛼 − 𝑇0 )] With 𝜇∞ the infinite shear viscosity, 𝜇0 the zero shear viscosity, 𝑛 the power law index, 𝜆 a time constant, 𝛼 the activation energy, 𝑇0 the initial temperature, 𝑇 the temperature at any given time 𝑡 and 𝑇𝛼 the reference temperature at which 𝐻(𝑇) = 1. *ICFD_MODEL_NONNEWT 𝜇 = 𝜇0 1 + (𝜆𝛾̇)1−𝑛 With 𝜇0 the zero shear viscosity, 𝑛 the power law index and 𝜆 a time constant. d) HERSCHEL-BULKLEY : 𝜇 = 𝜇0 𝑖𝑓 (𝛾̇ < 𝜏0 𝜇0⁄ ) 𝜇 = 𝜏0 + 𝑘[𝛾̇ 𝑛 − (𝜏0 𝜇0⁄ )𝑛] 𝛾̇ With 𝑘 the consistency index, 𝜏0 the Yield stress threshold, 𝜇0 the yielding vis- cosity and 𝑛 the power law index. e) CROSS II : 𝜇 = 𝜇∞ + 𝜇0 − 𝜇∞ 1 + (𝜆𝛾̇)𝑛 With 𝜇0 the zero shear viscosity, 𝜇∞ the infinite shear viscosity, 𝑛 the power law index and 𝜆 a time constant. 2. For the temperature dependent viscosity models, the viscosity is expressed as : a) SUTHERLAND’s LAW : 𝜇 = 𝜇0( 𝑇0 )3/2 𝑇0 + 𝑆 𝑇 + 𝑆 With 𝜇0 a reference viscosity, 𝑇0 the initial temperature (which therefore must not be 0.), 𝑇 the temperature at any given time 𝑡 and 𝑆 Sutherland’s constant. b) POWER LAW : 𝜇 = 𝜇0( 𝑇0 )𝑛 With 𝜇0 a reference viscosity, 𝑇0 the initial temperature (which therefore must not be 0.), 𝑇 the temperature at any given time 𝑡 and 𝑛 the power law index. 3. For NNID = 8, a load curve, a load curve function or a function can be used. If it references a DEFINE_FUNCTION, the following arguments are allowed 𝑓 (𝑥, 𝑦, 𝑧, 𝑣𝑥, 𝑣𝑦, 𝑣𝑧, 𝑡𝑒𝑚𝑝 , 𝑝𝑟𝑒𝑠, 𝑠ℎ𝑒𝑎𝑟, 𝑡𝑖𝑚𝑒). Purpose: Specify a porous media model. Porous Media Model ID and type. *ICFD Card 1 1 2 3 4 5 6 7 8 Variable PMMOID PMID Type I I Default none none Porous Media Parameters Card. Card 2 1 2 3 4 5 6 7 8 Variable POR PER/THX FF/THY THZ PVLCIDX PVLCIDY PVLCIDZ Type F Default 0. F 0. F 0. F I I I 0. none none none Permeability Vector Card in local reference frame. Only to be defined if the porous media is anisotropic. 4 5 6 7 8 Card 3 1 Variable KX’ Type F Default 0. 2 KY’ F 0. 3 KZ’ F 0. Projection of local Vectors in global reference frame. Only to be defined if the porous media is anisotropic. Card 4 1 2 3 Variable 1-X/1-PID 1-Y/2-PID 1-Z 4 2-X 5 2-Y 6 2-Z 7 8 Type F/I F/I F/I F/I F/I F/I Default 0 0. 0. 0. 0. 0. VARIABLE DESCRIPTION PMMOID Porous media model ID. PMID Porous media model type : EQ.1 : Isotropic porous media - Ergun Correlation. EQ.2 : Isotropic porous media - Darcy-Forchheimer model. EQ.3 : Isotropic porous media - Permeability defined through Pressure-Velocity Data. EQ.4 : Anisotropic porous media - Fixed local reference frame . EQ.5 : Anisotropic porous media model - Moving local reference frame and permeability vector in local reference frame (𝑥’, 𝑦’, 𝑧’) defined by three Pressure-Velocity curves. EQ.6 : Anisotropic porous media model - Moving local reference frame and permeability vector constant. EQ.7: Anisotropic porous media model - Moving local reference frame and permeability vector constant. This model dif- fers from PMID = 6 in the way the local reference frame is moved. POR Porosity 𝜀. PER/THX FF/THY Permeability 𝜅 if PMID = 1 or 2. Probe Thickness ∆𝑥 if PMID = 3 or PMID = 5. Forchheimer factor. To Be defined if PMID = 2. Probe Thickness ∆𝑦 if PMID = 5. THZ Probe Thickness ∆𝑧 if PMID = 5. DESCRIPTION Pressure function of Velocity Load Curve ID. To be defined if PMID = 3 and PMID = 5. If PMID = 5, this refers to P-V curve in global X direction. For PMID = 1 and PMID = 2, this flags acts as an optional load curve ID, define curve function ID or define function ID. If a DEFINE_FUNCTION is used, the following parameters are allowed: 𝑓 (𝑥, 𝑦, 𝑧, 𝑣𝑥, 𝑣𝑦, 𝑣𝑧, 𝑡𝑒𝑚𝑝, 𝑝𝑟𝑒𝑠, 𝑡𝑖𝑚𝑒). Pressure function of Velocity Load Curve ID. To be defined if PMID = 5. This refers to P-V curve in global Y direction. Pressure function of Velocity Load Curve ID. To be defined if PMID = 5. This refers to P-V curve in global Z direction. Permeability vector in local reference frame (𝑥’, 𝑦’, 𝑧’). To be defined in PMID = 4, 5, 6 or 7. Those values become scale factors if PMID = 5. Projection of local permeability vector 𝐱’ in global reference frame (𝑥, 𝑦, 𝑧). To be defined if PMID = 4. If PMID = 6, those become load curve IDs so the coordinates of the local 𝐱’ vector can be made to move through time. Projection of local permeability vector 𝐲’ in global reference frame (𝑥, 𝑦, 𝑧). To be defined if PMID = 4. If PMID = 6, those become load curve IDs so the coordinates of the local 𝐲’ vector can be made to move through time. If PMID = 5 or PMID = 7, the two local reference frame vectors are defined by the coordinates of the two point IDs defined by 1-PID and 2-PID. . Since those points can be made to move, it is therefore possible to define a moving reference frame for the anisotropic porous media domain. VARIABLE PVLCIDX PVLCIDY PVLCIDZ KX’/KY’/KZ’ 1-X/1-Y/1-Z 2-X/2-Y/2-Z 1-PID/2-PID Remarks: 1. Being 𝜀 the porosity and 𝜅 the permeability of the porous media respectively, one can define: 𝜀 = 𝑣𝑜𝑖𝑑 𝑣𝑜𝑙𝑢𝑚𝑒 𝑡𝑜𝑡𝑎𝑙 𝑣𝑜𝑙𝑢𝑚𝑒 And being 𝑢𝑖 the volume averaged velocity field defined in terms of the fluid ve- locity field 𝑢𝑖𝑓 as: y' x' Figure 5-6. Anisotropic porous media vectors definition (PMID = 4,5,6,7). The vectors 𝐗 and 𝐘 are the global axes; 𝐱′ and 𝐲′ define system for the primed coordinate(𝑥′, 𝑦′, 𝑧′). 𝑢𝑖 = 𝜀𝑢𝑖𝑓 The generalized flow equations of momentum and mass conservation can be ex- pressed as : 𝜕𝑢𝑖 𝜕𝑥𝑖 = 0 𝜀 [ 𝜕𝑢𝑖 𝜕𝑡 + 𝜕 𝜕𝑥𝑗 𝜕𝑢𝑖𝑢𝑗 𝜀 )] = − 1 ( 𝜕(𝑃𝜀) 𝜕𝑥𝑖 + 𝜀 ( 𝜕2𝑢𝑖 𝜕𝑥𝑗𝜕𝑥𝑗 ) + 𝜌𝑔𝑖 − 𝐷𝑖 Where 𝐷𝑖 are the forces exerted to the fluid by the porous matrix. For the isotropic model, the porous forces are a function of the matrix porosity and its permeability. For the isotropic case, three models are available : a) Model 1 : Ergun correlation 𝐷𝑖 = b) Model 2 : Darcy-Forcheimer 𝐷𝑖 = 𝜇𝑢𝑖 𝜅 + 1.75𝜌|𝑈| √150√𝜅𝜀3/2 𝑢𝑖 𝜇𝑢𝑖 𝜅 + 𝐹𝜀𝜌|𝑈| √𝜅 𝑢𝑖 c) Model 3 : Using the 𝛥𝑃 − 𝑉 experimental data. In this case, it is assumed that the pressure velocity curve was obtained applying a pressure differ- ence or pressure drop on both ends of a porous slab of thickness 𝛥𝑥 with porous properties 𝜅 and 𝜀. It then becomes possible for the solver to fit that experimental curve with a quadratic polynomial of the form 𝛥𝑃(𝑢𝑥) = 𝛼𝑢𝑥 2 + 𝛽𝑢𝑥. Once 𝛼 and 𝛽 are known, it is possible to estimate 𝐷𝑖. 2. The anisotropic version of the Darcy-Forcheimer term can be written as : 𝐷𝑖 = 𝜇𝐵𝑖𝑗𝜇𝑗 + 𝐹𝜀|𝑈|𝐶𝑖𝑗𝑢𝑗 𝐵𝑖𝑗 = (𝐾𝑖𝑗) −1 𝐶𝑖𝑗 = (𝐾𝑖𝑗) −1/2 Where 𝐾𝑖𝑗 is the anisotropic permeability tensor. Available options include TITLE *ICFD_PART Purpose: Define parts for this incompressible flow solver. The TITLE option allows the user to define an additional optional line with a HEADING in order to associate a name to the part. Card 1 1 2 3 4 5 6 7 8 Variable Type Default HEADING A none Part Material Card. Include as many cards as needed. This input ends at the next keyword (“*”) card. Card 2 1 2 3 4 5 6 7 8 Variable PID SECID MID Type I I I Default none none none VARIABLE DESCRIPTION PID Part identifier for fluid surfaces. SECID Section identifier defined with the *ICFD_SECTION card. MID Material identifier defined with the *ICFD_MAT card. Available options include TITLE *ICFD Purpose: This keyword assigns material properties to the nodes enclosed by surface ICFD parts. The TITLE option allows the user to define an additional optional line with a HEADING in order to associate a name to the part. Title 1 2 3 4 5 6 7 8 Variable Type Default HEADING A none Card 1 1 2 3 4 5 6 7 8 Variable PID SECID MID Type I I I Default none none none Provide as many cards as necessary. This input ends at the next keyword (“*”) card Card 2 1 2 3 4 5 6 7 8 Variable SPID1 SPID2 SPID3 SPID4 SPID5 SPID6 SPID7 SPID8 Type I I I I I I I I Default none none none none none none none none *ICFD_PART_VOL DESCRIPTION PID Part identifier for fluid volumes. SECID Section identifier defined by the *ICFD_SECTION card. MID Material identifier. SPID1, … Part IDs for the surface elements that define the volume mesh. PID 3 PID 4 PID 5 PID 3 $$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ $$$$ *ICFD_PART_VOL $$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ $ $ PART ID 5 is defined by the surfaces that enclose it. $ *ICFD_PART_VOL $ $...>....1....>....2....>....3....>....4....>....5....>....6....>....7....>....8 $ pid secid mid 5 1 1 $...>....1....>....2....>....3....>....4....>....5....>....6....>....7....>....8 $ pid1 pid2 pid3 pid4 pid5 pid6 pid7 pid8 1 2 3 4 *ICFD Purpose: Define a section for the incompressible flow solver. Card 1 1 2 3 4 5 6 7 8 Variable SID Type I Default none VARIABLE DESCRIPTION SID Section identifier. *ICFD_SET_NODE_LIST Purpose: Only used in cases where the mesh is specified by the user . Defines a set of nodes associated with a part ID on which boundary conditions can be applied. 3 4 5 6 7 8 Card 1 1 Variable SID 2 PID Type I I Default none none Node List Card. Provide as many cards as necessary. This input ends at the next keyword (“*”) card Card 2 1 2 3 4 5 6 7 8 Variable NID1 NID2 NID3 NID4 NID5 NID6 NID7 NID8 Type I I I I I I I I Default none none none none none none none none VARIABLE DESCRIPTION SID PID Set ID Associated Part ID. NID1, … Node IDs Remarks: 1. The convention is the similar to the one used by the keyword *SET_NODE_LIST and serves a similar purpose. *ICFD Purpose: This keyword provides an option to trigger an iterative procedure on the fluid system. This procedure aims to bring more precision to the final pressure and velocity values but is often very time consuming. It must therefore be used with caution. It is intended only for special cases. For stability purposes, this method is automatically used for the first ICFD time step. Card 1 1 2 3 4 5 6 7 8 Variable NIT TOL Type Default I 1 F 10-3 VARIABLE DESCRIPTION NIT TOL Maximum Number of iterations of the system for each fluid time step. If TOL criteria is not reached after NIT iterations, the run will proceed. Tolerance Criteria for the pressure residual during the fluid system solve. *ICFD_SOLVER_TOL_MMOV Purpose: This keyword allows the user to change the default tolerance values for the mesh movement algorithm. Care should be taken when deviating from the default values. Card 1 1 2 3 4 5 6 7 8 Variable ATOL RTOL MAXIT Type F F I Default 1e-8 1e-8 1000 VARIABLE ATOL RTOL MAXIT DESCRIPTION Absolute convergence criteria. Convergence is achieved when Residual𝑖+1 − Residual𝑖 ≤ ATOL. If a negative integer is entered, then that value will be used as a load curve ID for ATOL. Relative convergence criteria. Convergence is achieved when (Residual𝑖+1 − Residual𝑖) Residualinitial ≤ RTOL. If a negative integer is entered, then that value will be used as a load curve ID for RTOL. ⁄ Maximum number of iterations allowed to achieve convergence. If a negative integer is entered, then that value will be used as a load curve ID for MAXIT. *ICFD Purpose: This keyword allows the user to change the default tolerance values for the momentum equation solve. Care should be taken when deviating from the default values. Card 1 1 2 3 4 5 6 7 8 Variable ATOL RTOL MAXIT Type F F I Default 10-8 10-8 1000 VARIABLE ATOL RTOL MAXIT DESCRIPTION Absolute convergence criteria. Convergence is achieved when Residual𝑖+1 − Residual𝑖 ≤ ATOL. If a negative integer is entered, then that value will be used as a load curve ID for ATOL. Relative convergence criteria. Convergence is achieved when (Residual𝑖+1 − Residual𝑖) Residualinitial ≤ RTOL. If a negative integer is entered, then that value will be used as a load curve ID for RTOL. ⁄ Maximum number of iterations allowed to achieve convergence. If a negative integer is entered, then that value will be used as a load curve ID for MAXIT. *ICFD_SOLVER_TOL_MONOLITHIC Purpose: This keyword allows the user to change the default tolerance values for the monolithic solver. Care should be taken when deviating from the default values. Card 1 1 2 3 4 5 6 7 8 Variable ATOL RTOL MAXIT Type F F I Default 10-8 10-8 1000 VARIABLE ATOL RTOL MAXIT DESCRIPTION Absolute convergence criteria. Convergence is achieved when Residual𝑖+1 − Residual𝑖 ≤ ATOL. If a negative integer is entered, then that value will be used as a load curve ID for ATOL. Relative convergence criteria. Convergence is achieved when (Residual𝑖+1 − Residual𝑖) Residualinitial ≤ RTOL. If a negative integer is entered, then that value will be used as a load curve ID for RTOL. ⁄ Maximum number of iterations allowed to achieve convergence. If a negative integer is entered, then that value will be used as a load curve ID for MAXIT. *ICFD Purpose: This keyword allows the user to change the default tolerance values for the Poisson equation for pressure. Care should be taken when deviating from the default values. Card 1 1 2 3 4 5 6 7 8 Variable ATOL RTOL MAXIT Type F F I Default 10-8 10-8 1000 VARIABLE ATOL RTOL MAXIT DESCRIPTION Absolute convergence criteria. Convergence is achieved when Residual𝑖+1 − Residual𝑖 ≤ ATOL. If a negative integer is entered, then that value will be used as a load curve ID for ATOL. Relative convergence criteria. Convergence is achieved when (Residual𝑖+1 − Residual𝑖) Residualinitial ≤ 𝑅𝑇𝑂𝐿. If a negative integer is entered, then that value will be used as a load curve ID for RTOL. ⁄ Maximum number of iterations allowed to achieve convergence. If a negative integer is entered, then that value will be used as a load curve ID for MAXIT. *ICFD_SOLVER_TOL_TEMP Purpose: This keyword allows the user to change the default tolerance values for the heat equation. To be handled with great care. Card 1 1 2 3 4 5 6 7 8 Variable ATOL RTOL MAXIT Type F F I Default 1e-8 1e-8 1000 VARIABLE ATOL RTOL MAXIT DESCRIPTION Absolute convergence criteria. Convergence is achieved when 𝑅𝑒𝑠𝑖𝑑𝑢𝑎𝑙𝑖+1 − 𝑅𝑒𝑠𝑖𝑑𝑢𝑎𝑙𝑖 ≤ 𝐴𝑇𝑂𝐿. If a negative integer is entered, then that value will be used as a load curve ID for ATOL. Relative convergence criteria. Convergence is achieved when (𝑅𝑒𝑠𝑖𝑑𝑢𝑎𝑙𝑖+1 − 𝑅𝑒𝑠𝑖𝑑𝑢𝑎𝑙𝑖) 𝑅𝑒𝑠𝑖𝑑𝑢𝑎𝑙𝑖𝑛𝑖𝑡𝑖𝑎𝑙 ≤ 𝑅𝑇𝑂𝐿. If a negative integer is entered, then that value will be used as a load curve ID for RTOL. ⁄ Maximum number of iterations allowed to achieve convergence. If a negative integer is entered, then that value will be used as a load curve ID for MAXIT. *MESH The keyword *MESH is used to create a mesh that will be used in the analysis. So far only tetrahedral (or triangular in 2-d) elements can be generated. The keyword cards in this section are defined in alphabetical order: *MESH_BL *MESH_BL_SYM *MESH_EMBEDSHELL *MESH_INTERF *MESH_NODE *MESH_SIZE *MESH_SIZE_SHAPE *MESH_SURFACE_ELEMENT *MESH_SURFACE_NODE *MESH_VOLUME *MESH_VOLUME_ELEMENT *MESH_VOLUME_NODE *MESH_VOLUME_PART An additional option “_TITLE” may be appended to all *MESH keywords. If this option is used, then an 80 character string is read as a title from the first card of that keyword's input. At present, LS-DYNA does not make use of the title. Inclusion of titles gives greater clarity to input decks. *MESH_BL Purpose: This keyword is used to define a boundary-layer mesh as a refinement on volume-mesh. The boundary layer mesh is constructed by subdividing elements near the surface. Boundary Layer Cards. Define as many cards as are necessary. The next “*” card terminates the input. Card 1 1 2 3 4 5 6 7 8 Variable PID NELTH BLTH BLFE BLST Type I I F Default none none 0. F 0. I 0 VARIABLE DESCRIPTION PID Part identifier for the surface element. NELTH BLTH BLFE Number of elements normal to the surface (in the boundary layer) is NELTH+1. Boundary layer mesh thickness if BLST = 1 or BLST = 2. Growth scale factor if BLST = 3. Ignored if BLST = 0. Distance between the wall and the first volume mesh node. Not used if BLST = 0 or BLST = 1. BLST Boundary layer mesh generation strategy : EQ.0: By default, for every additional NELTH, the automatic volume mesher will divide the elements closest to the sur- face by two so that the smallest element in the boundary layer mesh will have an aspect ratio of 2NELTH+1. A default boundary layer mesh thickness based on the surface mesh size will be chosen. EQ.1: Constant repartition using BLFE and NELTH. EQ.2: Repartition following a quadratic polynomial. EQ.3: Repartition following a growth scale factor. *MESH 1. For BLST = 1, the distance between the wall and the first node will be equal to 𝐵𝐿𝑇𝐻 (𝑁𝐸𝐿𝑇𝐻 + 1) ⁄ . 2. For BLST = 3, the total thickness of the boundary layer will be equal to ∑ 𝑁𝐸𝐿𝑇𝐻 𝑛=0 𝐵𝐿𝐹𝐸 × 𝐵𝐿𝑇𝐻𝑛 . *MESH_BL_SYM Purpose: Specify the part IDs that will have symmetry conditions for the boundary layer. On these surfaces, the boundary layer mesh follows the surface tangent. Boundary Layer with Symmetry Condition Cards. Define as many cards as necessary. The next “*” card terminates the input. Card 1 1 2 3 4 5 6 7 8 Variable PID1 PID2 PID3 PID4 PID5 PID6 PID7 PID8 Type I I I I I I I I Default none none none none none none none none VARIABLE PID1, … DESCRIPTION Part identifiers for the surface element. This is the surface with symmetry. *MESH Purpose: Define surfaces that the mesher will embed inside the volume mesh. These surfaces will have no thickness and will conform to the rest of the volume mesh having matching nodes on the interface. Card 1 1 2 3 4 5 6 7 8 Variable VOLID Type I Default none Define as many cards as are necessary based on the number of PIDs (the next “*” card terminates the input.) Card 2 1 2 3 4 5 6 7 8 Variable PID1 PID2 PID3 PID4 PID5 PID6 PID7 PID8 Type I I I I I I I I Default none none none none none none none none VARIABLE DESCRIPTION VOLID PIDn ID assigned to the new volume in the keyword *MESH_VOLUME. The surface mesh size will be applied to this volume. Part IDs for the surface elements that will be embedded in the volume mesh. *MESH_INTERF Purpose: Define the surfaces that will be used by the mesher to specify fluid interfaces in multi-fluid simulations. Card 1 1 2 3 4 5 6 7 8 Variable VOLID Type I Default none Define as many cards as are necessary based on the number of PIDs. This input ends at the next keyword (“*”) card. Card 2 1 2 3 4 5 6 7 8 Variable PID1 PID2 PID3 PID4 PID5 PID6 PID7 PID8 Type I I I I I I I I Default none none none none none none none none VARIABLE VOLID DESCRIPTION ID assigned to the new volume in the keyword *MESH_VOLUME. The interface meshes will be applied to this volume. PIDn Part IDs for the surface elements. *MESH Purpose: Define a fluid node and its coordinates. These nodes are used in the mesh generation process by the *MESH_SURFACE_ELEMENT keyword, or as user defined volume nodes by the *MESH_VOLUME_ELEMENT keyword. Node Cards. Include one additional card for each node. This input ends at the next keyword (“*”) card. Card 1 1 2 3 4 5 6 7 8 9 10 Variable NID Type I Default none X F 0 Y F 0 Z F 0 VARIABLE DESCRIPTION NID Node ID. A unique number with respect to the other surface nodes. X Y Z 𝑥 coordinate. 𝑦 coordinate. 𝑧 coordinate. Remarks: 1. The data card format for the *MESH_NODE keyword is identical to *NODE. 2. The *MESH_NODE keyword supersedes *MESH_SURFACE_NODE, which was for surfaces nodes as well as *MESH_VOLUME_NODE for, which was for volume nodes in user defined. *MESH_SIZE Purpose: Define the surfaces that will be used by the mesher to specify a local mesh size inside the volume. If no internal mesh is used to specify the size, the mesher will use a linear interpolation of the surface sizes that define the volume enclosure. Card 1 1 2 3 4 5 6 7 8 Variable VOLID Type I Default none Define as many cards as are necessary based on the number of PIDs (the next “*” card terminates the input.). Card 2 1 2 3 4 5 6 7 8 Variable PID1 PID2 PID3 PID4 PID5 PID6 PID7 PID8 Type I I I I I I I I Default none none none none none none none none VARIABLE DESCRIPTION VOLID PIDn ID assigned to the new volume in the keyword *MESH_VOLUME. The mesh sizing will be applied to this volume. Part IDs for the surface elements that are used to define the mesh size next to the surface mesh. *MESH Purpose: Defines a local mesh size in specific zones corresponding to given geometrical shapes (box, sphere, and cylinder). The solver will automatically apply the conditions specified during the generation of the volume mesh. This zone does not need to be entirely defined in the volume mesh. Remeshing Control Card sets: Add as many remeshing control cards paired with a case card as desired. The input of such pairs ends at the next keyword “*” card. Remeshing Control. First card specifies whether to maintain this mesh sizing criterion through a remesh operation. Card 1 1 2 3 4 5 6 7 8 Variable SNAME FORCE Type A Default none I 0 Box Case. Card 2 for SNAME = “box” Cards 2 1 2 3 4 5 6 7 8 Variable MSIZE PMINX PMINY PMINZ PMAXX PMAXY PMAXZ Type F F F F F F F Default none none none none none none none Sphere Case. Card 2 for SNAME = “sphere” Cards 2 1 2 3 4 5 6 7 8 Variable MSIZE RADIUS CENTERX CENTERY CENTERZ Type F F F F F Default none none none none none Cylinder Case. Card 2 for SNAME = “cylinder” Cards 2 1 2 3 4 5 6 7 8 Variable MSIZE RADIUS PMINX PMINY PMINZ PMAXX PMAXY PMAXZ Type F F F F F F F F Default none none none none none none none none VARIABLE SNAME DESCRIPTION Shape name. Possibilities include “box”, “cylinder” and “sphere” FORCE Force to keep the mesh size criteria even after a remeshing is done. EQ.0: Off, mesh size shape will be lost if a remeshing occurs EQ.1: On. MSIZE Mesh size that needs to be applied in the zone of the shape defined by SNAME PMIN[X, Y, Z] 𝑥, 𝑦, or 𝑧 value for the point of minimum coordinates PMAX[X, Y, Z] 𝑥, 𝑦, or 𝑧 value for the point of maximum coordinates CENTER[X, Y, Z] Coordinates of the sphere center in cases where SNAME is sphere RADIUS Radius of the sphere if SNAME is Sphere or of the cross section disk if SNAME is Cylinder. *MESH Purpose: Specify a set of surface elements (quadrilateral or triangular in 3-d and linear segments in 2-d) that will be used by the mesher to construct a volume mesh. These surface elements may be used to define the enclosed volume to be meshed, or alternatively they could be used to apply different mesh sizes inside the volume . Surface Element Card. Define as many cards as necessary. The next “*” card terminates the input. Card 1 1 2 Variable EID PID 3 N1 4 N2 5 N3 6 N4 7 8 9 10 Type I I I I I I Default none none none none none none VARIABLE DESCRIPTION Element ID. A unique number with respect to all *MESH_SUR- FACE_ELEMENTS cards. Mesh surface part ID. A unique identifier for the surface to which this mesh surface element belongs. Nodal point 1. Nodal point 2. Nodal point 3. Nodal point 4. EID PID N1 N2 N3 N4 Remarks: 1. The convention is the same used by the keyword *ELEMENT_SHELL. In the case of a triangular face N3 = N4. In 2-d N2 = N3 = N4. Note that the accepted card format is 6i8 (not 6i10) *MESH_SURFACE_NODE Purpose: Define a node and its coordinates. These nodes will be used in the mesh generation process by the *MESH_SURFACE_ELEMENT keyword. *MESH_NODE supersedes this card; so please use *MESH_NODE instead of this card. Surface Node Cards. Include one card for each node. Include as many cards a necessary. This input ends at the next keyword (“*”) card. Card 1 1 2 3 4 5 6 7 8 9 10 Variable NID Type I Default none X F 0 Y F 0 Z F 0 VARIABLE DESCRIPTION NID Node ID. This NID must be unique within the set of surface nodes. X Y Z 𝑥 coordinate. 𝑦 coordinate. 𝑧 coordinate. *MESH Purpose: This keyword defines the volume space that will be meshed. The boundaries of the volume are the surfaces defined by *MESH_SURFACE_ELEMENT. The surfaces listed have to be non-overlapping, and should not leave any gaps or open spaces between the surface boundaries. On the boundary between two neighbor surfaces, nodes have to be in common (no duplicate nodes) and should match exactly on the interface. They are defined by the keyword *MESH_SURFACE_NODE. This card will be ignored if the volume mesh is specified by the user and not generated automatically. Card 1 1 2 3 4 5 6 7 8 Variable VOLID Type I Default none Define as many cards as are necessary based on the number of PIDs (the next “*” card terminates the input.) Card 2 1 2 3 4 5 6 7 8 Variable PID1 PID2 PID3 PID4 PID5 PID6 PID7 PID8 Type I I I I I I I I Default none none none none none none none none VARIABLE DESCRIPTION VOLID ID assigned to the new volume. PIDn Part IDs for the surface elements that are used to define the volume. *MESH_VOLUME_ELEMENT Purpose: Specify a set of volume elements for the fluid volume mesh in cases where the volume mesh is specified by the user and not generated automatically. The nodal point are specified in the *MESH_VOLUME_NODE keyword. Only tetrahedral elements are supported (triangles in 2D). Volume Element Card. Define as many cards as necessary. The next “*” card terminates the input. Card 1 1 2 Variable EID PID 3 N1 4 N2 5 N3 6 N4 7 8 9 10 Type I I I I I I Default none none none none none none VARIABLE DESCRIPTION Element ID. A unique number with respect to all *MESH_VOL- UME_ELEMENTS cards. Part ID. A unique part identification number. Nodal point 1. Nodal point 2. Nodal point 3. Nodal point 4. EID PID N1 N2 N3 N4 Remarks: 1. The convention is the same used by the keyword *ELEMENT_SOLID. *MESH Purpose: Define a node and its coordinates. This keyword is only used in cases where the fluid volume mesh is provided by the user and is not automatically generated. It serves the same purpose as the *NODE keyword for solid mechanics. Only tetrahedral elements are supported. *MESH_NODE supersedes this card; so please use *MESH_NODE instead of this card. Volume Node Cards. Include as many cards in the following format as desired. This input ends at the next keyword (“*”) card. Card 1 1 2 3 4 5 6 7 8 9 10 Variable NID Type I Default none X F 0 Y F 0 Z F 0 VARIABLE DESCRIPTION NID Node ID. A unique number with respect to the other volume nodes. X Y Z 𝑥 coordinate. 𝑦 coordinate. 𝑧 coordinate. *MESH_VOLUME_PART Purpose: Associate a volume part number created by a *MESH_VOLUME card with the part number of a part card from a selected solver (designated by the SOLVER field). Mesh Volume Part Card. Include as many cards in the following format as desired. This input ends at the next keyword (“*”) card. Card 1 1 2 3 4 5 6 7 8 Variable VOLPRT SOLPRT SOLVER Type I I A Default VARIABLE DESCRIPTION VOLPRT Part ID of a volume part created by a *MESH_VOLUME card. SOLPRT Part ID of a part created using SOLVER’s part card. SOLVER Name of a solver using a mesh created with *MESH cards. *STOCHASTIC The keyword *STOCHASTIC is used to describe the particles and numerical details for solving a set of stochastic PDEs. Currently, there are two types of stochastic PDE models in the code: a model of embedded particles in TBX explosives, and a spray model. The cards for using these models are: *STOCHASTIC_SPRAY_PARTICLES *STOCHASTIC_TBX_PARTICLES An additional option “_TITLE” may be appended to all *STOCHASTIC keywords. If this option is used, then an 80 character string is read as a title from the first card of that keyword's input. At present, LS-DYNA does not make use of the title. Inclusion of titles gives greater clarity to input decks. *STOCHASTIC_SPRAY_PARTICLES Purpose: Specify particle and other model details for spray modeling using stochastic PDEs that approximate such processes. A pair of cards is required to specify the characteristics of each nozzle (cards 3 and 4 describe the first nozzle). Card 1 1 2 3 4 5 6 7 8 Variable INJDIST IBRKUP ICOLLDE IEVAP IPULSE LIMPR IDFUEL Type Default I 1 I I none none Card 2 1 2 3 I 0 4 I I none none 5 6 I 1 7 8 Variable RHOP TIP PMASS PRTRTE STRINJ DURINJ Type F F F F F F Nozzle card 1: Provide as many pairs of nozzle cards 1 and 2 as necessary. This input ends at the next keyword (“*”) card (following a nozzle card 2). Card 3 1 2 3 4 5 6 7 8 Variable XORIG YORIG ZORIG SMR VELINJ DRNOZ DTHNOZ Type F F F F F F Nozzle card 2: Provide as many pairs of nozzle cards 1 and 2 as necessary. This input ends at the next keyword (“*”) card. Card 4 1 2 3 4 5 6 7 8 Variable TILTXY TILTXZ CONE DCONE ANOZ AMP0 Type F F F F F F VARIABLE DESCRIPTION INJDIST Spray particle size distribution: EQ.1: EQ.2: EQ.3: EQ.4: uniform Rosin-Rammler (default) Chi-squared degree of 2 Chi-squared degree of 6 IBRKUP Type of particle breakup model: EQ.0: EQ.1: EQ.2: off (no breakup) TAB KHRT ICOLLDE Turn collision modeling on or off IEVAP Evaporation flag: EQ.0: EQ.1: off (no evaporation) Turn evaporation on IPULSE Type of injection: EQ.0: EQ.1: EQ.2: continuous injection sine wave square wave LIMPRT Upper limit on the number of parent particles modeled in this spray. This is not used with the continuous injection case (IPULSE = 0). VARIABLE DESCRIPTION IDFUEL Selected spray liquid fuels: EQ.1: EQ.2: EQ.3: EQ.4: EQ.5: EQ.6: EQ.7: EQ.8: EQ.9: (Default), H2O Benzene, C6H6 Diesel # 2, C12H26 Diesel # 2, C13H13 Ethanol, C2H5OH Gasoline, C8H18 Jet-A, C12H23 Kerosene, C12H23 Methanol, CH3OH EQ.10: N-dodecane, C12H26 RHOP Particle density TIP Initial particle temperature. PMASS Total particle mass PRTRTE Number of particles injected per second for continuous injection. STRINJ Start of injection(s) DURINJ Duration of injection(s) XORIG X-coordinate of center of a nozzle’s exit plane YORIG Y-coordinate of center of a nozzle’s exit plane ZORIG Z-coordinate of center of a nozzle’s exit plane SMR Sauter mean radius VELINJ Injection velocity DRNOZ Nozzle radius DTHNOZ Azimuthal angle (in degrees measured counterclockwise) of the injector nozzle from the j = 1 plane. VARIABLE TILTXY DESCRIPTION Rotation angle (in degrees) of the injector in the x-y plane, where 0.0 points towards the 3 o’clock position (j = 1 line), and the angle increases counterclockwise from there. TILTXZ Inclination angle (in degrees) of the injection in the x-z plane, where 0.0 points straight down, x > 0.0 points in the positive x direction, and x < 0.0 points in the negative x direction. CONE Spray mean cone angle (in degrees) for hollow cone spray; spray cone angle (in degrees) for solid cone spray. DCONE Injection liquid jet thickness in degrees. ANOZ Area of injector AMP0 Initial amplitude of droplet oscillation at injector Remarks: 1. When IEVAP = 1, the keyword input file must be modified in a fashion similar to a chemistry problem. This is illustrated in a portion of an example keyword file below. That is, the following keywords need to be used, along with the inclusion of other chemistry-related files (i.e. evap.inp and the corresponding thermody- namics data file): *CHEMISTRY_MODEL *CHEMISTRY_COMPOSITION *CHEMISTRY_CONTROL_FULL *CESE_INITIAL_CHEMISTRY $ Setup stochastic particles $ *STOCHASTIC_SPRAY_PARTICLES $ injdist ibrkup icollide ievap ipulse limprt fuelid 3 1 0 1 0 100000 1 $ rhop tip pmass[Kg] prtrte str_inj dur_inj 1000.0 300. 0.01 1.0e7 0.0 10.0 $ the next card is needed for fireball position and max. particle velocity: $ XORIG YORIG ZORIG SMR Velinj Drnoz Dthnoz 0.005 0.005 1.0e-5 5.0e-6 200.0 9.0e-5 $ TILTXY TILTXZ CONE DCONE ANOZ AMP0 0.0 0.0 15.0 15.0 2.5e-8 0.0 $ *CHEMISTRY_MODEL $ model_id jacsel errlim 10 1 0.0 evap.inp therm.dat tran.dat $ *CHEMISTRY_COMPOSITION $ comp_id model_id 11 10 $ molefra Species 1.0 O2 3.76 N2 $ *CHEMISTRY_CONTROL_FULL $ sol_id errlim 5 $$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$ $ $ Set global initial conditions for fluid $ *CESE_INITIAL_CHEMISTRY $ sol_id comp_id 5 11 $INITIAL CONDITIONS $ uic vic wic ric pic tic hic 0.0 0.0 0.0 1.2 101325. 300.0 0.0 *STOCHASTIC_TBX_PARTICLES Purpose: Specify particle and other model details for stochastic PDEs that model embedded particles in TBX explosives. Note that the components listed on the corresponding *CHEMISTRY_COMPOSITION card are in terms of molar concentrations of the species (in units of moles/[length]3, where “[length]” is the user’s length unit). For further information on the theory of the TBX model that has been implemented, a document on this topic can be found at this URL: http://www.lstc.com/applications/cese_cfd/documentation Card 1 1 2 3 4 5 6 7 8 Variable PCOMB NPRTCL MXCNT PMASS SMR RHOP TICP T_IGNIT Type Default I 0 I I F F F F F none none none none none none none Card 2 1 2 3 4 5 6 7 8 Variable INITDST AZIMTH ALTITD CPS/CVS HVAP EMISS BOLTZ Type Default I 1 Remarks F F F F F F none none none none none none 1 6 1 7 8 Card 3 1 2 3 4 5 Variable XORIG YORIG ZORIG XVEL YVEL ZVEL FRADIUS Type F F F F F F F Default none none none 0.0 0.0 0.0 none VARIABLE DESCRIPTION PCOMB Particle combustion model EQ.0: no burning EQ.1: K-model NPRTCL MXCNT Initial total number of parent particles (discrete particles for calculation) Maximum allowed number of parent particles (during the simulation) PMASS Total particle mass SMR Sort mean particle radius RHOP Particle density TICP Initial particle temperature T_IGNIT Particle ignition temperature INITDST Initial particle distribution EQ.1: spatially uniform EQ.2: Rosin-Rammler EQ.3: Chi-squared AZIMTH ALTITD Angle in degrees from 𝑥-axis in 𝑥-𝑦 plane of reference frame of TBX explosive (0 < AZMITH < 360) Angle in degrees from 𝑧-axis of reference frame of TBX explosive (0 < ALTITD < 180) CPS/CVS Heat coefficient HVAP EMISS Latent heat of vaporization Particle emissivity BOLTZ Boltzmann coefficient XORIG 𝑥-coordinate of the origin of the initial reference frame of the TBX explosive VARIABLE DESCRIPTION YORIG ZORIG XVEL YVEL ZVEL 𝑦-coordinate of the origin of the initial reference frame of the TBX explosive 𝑧-coordinate of the origin of the initial reference frame of the TBX explosive 𝑥-component of the initial particle velocity the TBX explosive 𝑦-component of the initial particle velocity the TBX explosive 𝑧-component of the initial particle velocity the TBX explosive FRADIUS Radius of the explosive area. Remarks: 1. If radiation heat transfer is being modeled, then EMISS and BOLTZ are required. *LSO These cards provide a general data output mechanism, causing the creation of a sequence of LSDA files. This facility is intended to allow several different time sequences of data to be output in the same simulation. In addition, any number of domains (and any number of variables on those domains) may be specified within each time sequence. The keyword cards in this section are defined in alphabetical order: *LSO_DOMAIN *LSO_ID_SET (not available in the single-precision version of LS-DYNA) *LSO_POINT_SET *LSO_TIME_SEQUENCE *LSO_VARIABLE_GROUP Note that only the mechanics solver is available in the single-precision version of LS- DYNA, and therefore, only LSO mechanics variables are available for output from single precision LS-DYNA. These mechanics variables are listed by domain type in a separate document. This document (LSO_VARIABLES.TXT) is created by running the command: LS-DYNA print_lso_doc. Contrary to LSO_VARIABLES.TXT, element quantities such as stress are not available for output from the mechanics solver to the “lso” database. An additional option “_TITLE” may be appended to all *LSO keywords. If this option is used, then an 80 character string is read as a title from the first card of that keyword's input. At present, LS-DYNA does not make use of the title. Inclusion of titles gives greater clarity to input decks. *LSO_DOMAIN Purpose: This command provides a way to specify variables on a subset of the domain for a given solver. This domain can be a subset of the mesh used by that solver, a set of output points created with *LSO_POINT_SET, or a set of objects created with *LSO_ID_SET. The frequency and duration of the output for any given domain is determined by each *LSO_- TIME_SEQUENCE card that references this *LSO_DOMAIN card. Note that for the single- precision version of LS-DYNA, the only allowed value of SOLVER_NAME = MECH. Card 1 1 2 3 4 5 6 7 8 Variable Type DOMAIN_TYPE A Card 2 1 2 3 4 5 6 7 8 Variable Type SOLVER_NAME A Special Domains Card. Card 3 when DOMAIN_TYPE is one of ROGO, CIRCUIT, THIST_POINT or TRACER_POINT. Card 3 1 2 3 4 5 6 7 8 Variable OUTID REFID REDUCT Type I I I Default none none none Miscellaneous Domain Card. Card 3 when DOMAIN_TYPE is one of NODE, PART, SEG- MENT, SURFACE_NODE, SURFACE_ELEMENT, VOLUME_ELEMENT, SURFACE_- PART, VOLUME_PART. Card 3 1 2 3 4 5 6 7 8 Variable OUTID REFID OVERRIDE REDUCT Type I Default none I 0 I 0 I none Variable Name Card. Provide as many cards as necessary. This input ends at the next keyword (“*”) card Card 4 1 2 3 4 5 6 7 8 Variable Type VARIABLE_NAME A VARIABLE DESCRIPTION DOMAIN_TYPE The type of domain for which LSO output may be generated. SOLVER_NAME Selects the solver from which data is output on this domain. Accepted entries so far are “MECH”, “EM”, “CESE”, and “ICFD”. OUTID REFID LSO domain ID associated with this domain, and used by *LSO_TIME_SEQUENCE cards. Support set ID. This can be a set defined by a *SET card, a *LSO_ID_SET, card, or a *LSO_POINT_SET card. Unless OVERRIDE is specified, this set must be of the same type as DOMAIN_TYPE. OVERRIDE If non-zero, then REFID is interpreted as: EQ.1: a PART set for SOLVER_NAME EQ.2: a PART set of volume parts created with a *LSO_- ID_SET card (volume parts are defined with *MESH_VOLUME cards). EM ICFD CESE magneticField_point electricField_point vecpotField_point currentDensity2_point ScalarPotential_point velocity_point velocity_point pressure_point pressure_point temperature_point temperature_point density_point density_point lset_point Table 8-1. Selected LSO Varriables VARIABLE DESCRIPTION REDUCT EQ.3: a PART set of surface parts created with a *LSO_ID_- SET card (surface parts are defined with *MESH_- SURFACE_ELEMENT cards). EQ.4: a set of segment sets created with a *LSO_ID_SET card. A function that operates on the entire domain and returns a single value for scalar variables, three values for vector variables, or 6 values for symmetric tensor variables. For REDUCT=“range”, the number of returned values doubles. The following are the supported functions: EQ.BLANK: no reduction (default) EQ.“none”: Same as above EQ.“avg”: the average by component EQ.“average”: Same as above EQ.“min”: the minimum by component EQ.“minimum”: Same as above EQ.“max”: the maximum by component EQ.“maximum”: Same as above EQ.“sum”: the sum by component EQ.“range”: the minimum by component followed by *LSO DESCRIPTION the maximum by component VARIABLE_NAME Either the name of a single output variable or a variable group. See remarks. Remarks: 1. Supported choices for VARIABLE_NAME are listed by DOMAIN_TYPE for each SOLVER_NAME in a separate document. This document (LSO_VARIABLES.TXT) is created by running the command: LS-DYNA print_lso_doc. The following table shows a sample of the point output variables available when DOMAIN_- TYPE = THIST_POINT: *LSO_ID_SET Purpose: Provides a way to create a set of existing sets (segment sets), or to define a set that is not available with other set-related keyword cards. These are then used in other *LSO cards to specify LSO output. This card is not available in the single precision version of LS-DYNA. Card 1 1 2 3 4 5 6 7 8 Variable SETID TYPE SOLVER Type I A A Default none none MECH Referenced IDs. Provide as many cards as necessary. This input ends at the next keyword (“*”) card Card 1 Variable ID1 2 ID2 3 ID3 4 ID4 5 ID5 6 ID6 7 ID7 8 ID8 Type I I I I I I I I Default none none none none none none none none VARIABLE DESCRIPTION SETID Identifier for this ID set. DESCRIPTION TYPE The kind of IDs in this set: *LSO EQ.’SEG_SETS’: Each ID is a segment set connected with SOLVER. EQ.’CIRCUIT’: Each ID is a circuit ID (from *EM cards) EQ.’SURF_PARTS’: Each ID is a surface part number EQ.’VOL_PARTS’: Each ID is a volume part number EQ.’SURF_ELES’: Each ID is a surface element number SOLVER Name of the solver (MECH, ICFD, CESE, EM, …) ID1, … IDs of the TYPE kind. *LSO_POINT_SET Purpose: Define a list of points used to sample variables in time. Of the different sampling methods, the most common one is to specify points for time history output. Card 1 1 2 3 4 5 6 7 8 Variable SETID USE Type I Default none Remarks I 1 1 Point Cards. Provide as many cards as necessary. This input ends at the next keyword (“*”) card 4 5 6 7 8 Card Variable Type 1 X F 2 Y F 3 Z F Default none none none VARIABLE DESCRIPTION SETID Identifier for this point set. Used by *LSO_DOMAIN USE Points in this set are used as: EQ.1: Fixed time history points (default) EQ.2: Positions of tracer particles X, Y, Z Coordinates of a point. As many points as desired can be specified. *LSO 1. For USE = 1, with the ICFD and CESE solvers, the fixed points have to remain inside the fluid mesh or a zero result is returned, while for the EM solver, the points can be defined inside the conductors or in the air. In the latter case, the fields will be computed using a Biot-Savart type integration. For USE = 2, a mass- less tracer particle is tracked for the ICFD and CESE solvers using their local veloc- ity field to integrate the position of each particle in time. *LSO_TIME_SEQUENCE Purpose: This command provides users with maximum flexibility in specifying exactly what they want to have appear in the output LSO binary database. Each instance of the *LSO_TIME_SEQUENCE command creates a new time sequence with an independent output frequency and duration. Furthermore, while the default domain for each output variable will be the entire mesh on which that variable is defined, at all selected snapshot times, the *LSO_DOMAIN keyword commands can be used to specify that output will only occur on a portion of SOLVER_NAME’s mesh, and for a limited time interval, or that it will occur at a set of points , or over a set of object IDs . Note that for the single-precision version of LS-DYNA, the only allowed value of SOLVER_NAME = MECH. Card 1 1 2 3 4 5 6 7 8 Variable Type Card 2 Variable 1 DT Type F Default 0.0 Remarks 1 SOLVER_NAME A 2 3 4 5 6 7 8 LCDT LCOPT NPLTC TBEG TEND I 0 1 I 1 1 I 0 1 F F 0.0 0.0 Domain IDs. Provide as many cards as necessary. This input ends at the next keyword (“*”) card, or when a global variable name card appears Card 3 1 2 3 4 5 6 7 8 Variable DOMID1 DOMID2 DOMID3 DOMID4 DOMID5 DOMID6 DOMID7 DOMID8 Type I I I I I I I I Default none none none none none none none none Global variable names. Provide as many cards as necessary. This input ends at the next keyword (“*”) card Card 4 1 2 3 4 5 6 7 8 Variable Type GLOBAL_VAR A VARIABLE DESCRIPTION SOLVER_ NAME Selects the solver from which data is output in this time sequence. Accepted entries so far are ‘MECH’, ‘EM’, ‘CESE’ and ‘ICFD’ DT LCDT Time interval between outputs. Optional load curve ID specifying the time interval between dumps. LCOPT Flag to govern behavior of plot frequency load curve: EQ.1: At the time each plot is generated, the load curve value is added to the current time to determine the next plot time (this is the default behavior). EQ.2: At the time each plot is generated, the next plot time T is computed so that T = the current time plus the load curve value at the time T. EQ.3: A plot is generated for each ordinate point in the load curve definition. The actual value of the load curve is ignored. VARIABLE DESCRIPTION NPLTC DT = ENDTIM/NPLTC overrides DT specified in the first field. TBEG TEND The problem time at which to begin writing output to this time sequence The problem time at which to terminate writing output to this time sequence DOMID1, … Output set ID defining the domain over which variable output is to be performed in this time sequence. Each DOMID refers to the domain identifier in an *LSO_DOMAIN keyword card. The name of a global output variable computed by SOLVER_- NAME. This variable must have a single value (scalar, vector, or tensor), and therefore does not depend upon any DOMID. Any number of such variables may be specified with a given time sequence. These variables are listed as having “global” domain for SOLVER_NAME in a separate document. This document (LSO_VARIABLES.TXT) is created by running the command: LS- DYNA print_lso_doc. GLOBAL_VAR Remarks: 1. If LCDT is nonzero, then it is used and DT and NPLTC are ignored. If LCDT is zero and NPLTC is non-zero, then NPLTC determines the snapshot time incre- ment. If LCDT and NPLTC are both zero, then the minimum non-zero time in- crement specified by DT is used to determine the snapshot times. *LSO Purpose: To provide a means of defining a shorthand name for a group of variables. That is, wherever the given group name is used, it is replaced by the list of variables given in this command. Note that for the single-precision version of LS-DYNA, the only allowed value of SOLVER_NAME = MECH. Card 1 1 2 3 4 5 6 7 8 Variable Type SOLVER_NAME A Card 2 1 2 3 4 5 6 7 8 Variable Type DOMAIN_TYPE A Card 3 1 2 3 4 5 6 7 8 Variable Type GROUP_NAME A List Of Variables In Group. Provide as many cards as necessary. This input ends at the next keyword (“*”) card Card 4 1 2 3 4 5 6 7 8 Variable Type VAR_NAME A VARIABLE DESCRIPTION SOLVER_NAME Selects the solver for which data is output in a time sequence. DOMAIN_TYPE *LSO_VARIABLE_GROUP DESCRIPTION Name of the type of domain on which each VAR_NAME is defined. GROUP_NAME Name of (or alias for) the group of names given by the listed VAR_NAMEs VAR_NAME The name of an output variable computed by SOLVER_NAME Remarks: 1. Valid VAR_NAMEs depend both upon the SOLVER_NAME and the DOMAIN_- TYPE. These variables are listed by DOMAIN_TYPE for each SOLVER_NAME in a separate document. This document (LSO_VARIABLES.TXT) is created by run- ning the command: LS-DYNA print_lso_doc. Introduction This document presents some LS-DYNA examples providing a basic guide in different disciplines like: • Structural static (stress analysis, buckling analysis and modal analysis) • Structural dynamic (vibrations and impact) • Thermal analysis (heat transfer via conduction, convection and radiation) This guide is mainly addressed to first-time users. The input files are always present for each problem, using the KEYWORD input format. For sake of briefness, in most problems the full node and element definitions (also, some load segments) are omitted. Several of the problems present a closed-form solution, while others (the majority) a reference solution obtained by using an arbitrary refined mesh (NAFEMS Benchmarks). In these cases, the obtained value vs. the reference solution value is reported. Most of the problems are implicit ones. Problem-specific keywords are listed under the title of each problem. This guide refers to LS-DYNA v.971, but most of the problems also run on the 970, 960 and 950 versions. All problems have been tested using a double precision executable. Benchmark References Example 1. Skew Plate with Normal Pressure (thin shell mesh) The Standard NAFEMS Benchmarks, NAFEMS Report TNSB, Rev. 3, October, 1990, Test LE6. Example 2. Skew Plate with Normal Pressure (thick shell mesh) The Standard NAFEMS Benchmarks, NAFEMS Report TNSB, Rev. 3, October, 1990, Test LE6. Example 3. Elliptical Thick Plate under Normal Pressure (coarse mesh) Davies, G.A.O., Fenner, R.T., and Lewis, R.W., NAFEMS Background to Benchmarks, June, 1992, Test LE10. Example 4. Elliptical Thick Plate under Normal Pressure (fine mesh) Davies, G.A.O., Fenner, R.T., and Lewis, R.W., NAFEMS Background to Benchmarks, June, 1992, Test LE10. Example 5. Snap-Back under Displacement Control NAFEMS Non-Linear Benchmarks, NAFEMS Report NNB, Rev. 1, October, 1989, Test NL4. Example 6. Straight Cantilever Beam with Axial End Point Load NAFEMS Non-Linear Benchmarks, NAFEMS Report NNB, Rev. 1, October, 1989, Test NL6. Example 7. Lee's Frame Buckling Problem NAFEMS Non-Linear Benchmarks, NAFEMS Report NNB, Rev. 1, October, 1989, Test NL7. Example 8. Pin-Ended Double Cross: In-Plane Vibration The Standard NAFEMS Benchmarks, NAFEMS Report TNSB, Rev. 3, October, 1990, Test FV2. Example 9. Simply Supported Thin Annular Plate (coarse mesh) Abbassian, F., Dawswell, D.J., and Knowles, N.C., NAFEMS Selected Benchmarks for Natural Frequency Analysis, November, 1987, Test 14. Example 10. Simply Supported Thin Annular Plate (fine mesh) Abbassian, F., Dawswell, D.J., and Knowles, N.C., NAFEMS Selected Benchmarks for Natural Frequency Analysis, November, 1987, Test 14. Example 11. Transient Response to a Constant Force Example 12. Simply Supported Square Plate: Out-of Plane Vibration (solid mesh) Abbassian, F., Dawswell, D.J., and Knowles, N.C., NAFEMS Free Vibration Benchmarks, October, 2001, Test FV52. Example 13. Simply Supported Square Plate: Out-of-Plane Vibration (thick shell mesh) Abbassian, F., Dawswell, D.J., and Knowles, N.C., NAFEMS Free Vibration Benchmarks, October, 2001, Test FV52. Example 14. Simply Supported Square Plate: Transient Forced Vibration (solid mesh) Maguire, J., Dawswell, D.J., and Gould, L.,NAFEMS Selected Benchmarks for Forced Vibration, February, 1989, Test 21T. Example 15. Simply Supported Square Plate: Transient Forced Vibration (thick shell mesh) Maguire, J., Dawswell, D.J., and Gould, L., NAFEMS Selected Benchmarks for Forced Vibration, February, 1989, Test 21T. Example 16. Transient Response of a Cylindrical Disk Impacting a Deformable Surface Thomson, W.T., Vibration Theory and Applications, 2nd Printing, Prentice-Hall, Inc., Englewood Cliffs, New Jersey, 1965, pg. 110, ex. 4.6-1. Example 17. Natural Frequency of a Linear Spring-Mass System Timoshenko, S.P., and Young, D.H., Vibration Problems in Engineering, 3rd Edition, D. Van Nostrand Co., Inc., New York, New York, 1955, pg.1. Example 18. Natural Frequency of a Nonlinear Spring-Mass System Timoshenko, S.P., and Young, D.H., Vibration Problems in Engineering, 3rd Edition, D. Van Nostrand Co., Inc., New York, New York, 1955, pg. 141. Example 19. Buckling of a Thin Walled Cylinder Under Compression Timoshenko, S.P., and Gere, J.M., Theory of Elastic Stability, McGraw-Hill Book Co., Inc., New York, New York, 1961, pg. 457. Example 20. Membrane with a Hot Spot Davies, G.A.O., Fenner, R.T., and Lewis, R.W., NAFEMS Background to Benchmarks, June, 1992, Test T1. Example 21. 1D Transient Heat Transfer with Radiation Davies, G.A.O., Fenner, R.T., and Lewis, R.W., NAFEMS Background to Benchmarks, June, 1992, Test T2. Example 22. 1D Transient Heat Transfer in a Bar Example 23. 2D Heat Transfer with Convection Davies, G.A.O., Fenner, R.T., and Lewis, R.W., NAFEMS Background to Benchmarks, June, 1992, Test T4. Example 24. 3D Thermal Load Davies, G.A.O., Fenner, R.T., and Lewis, R.W., NAFEMS Background to Benchmarks, June, 1992, Test LE11. Example 25. Cooling of a Billet via Radiation Siegal, R., and Howell, J.R., Thermal Radiation Heat Transfer, 3rd Edition, Hemisphere Publishing Corporation, 1981, pg. 229, problem 21. Example 26. Pipe Whip Lerencz, R.M., Element-by-Element Preconditioning Techniques for Large-Scale, Vectorized Finite Element Analysis in Nonlinear Solid and Structural Mechanics, Ph.D. Thesis, Department of Mechanical Engineering, Stanford University, Palo Alto, California, March, 1989, pg. 142, pipe whip. Example 27. Aluminum Bar Impacting a Rigid Wall Lerencz, R.M., Element-by-Element Preconditioning Techniques for Large-Scale, Vectorized Finite Element Analysis in Nonlinear Solid and Structural Mechanics, Ph.D. 1. Skew Plate with Normal Pressure (thin shell mesh) Keywords: *CONTROL_IMPLICIT_GENERAL *CONTROL_IMPLICIT_SOLUTION Description: A skew plate of equal side lengths L and thickness t is subjected to a normal pressure P on the top face (Figure 1.1). The plate is meshed with thin shell elements with a 4 x 4 ZU = . Determine the density. The plate is simply supported on four side faces, maximum principal stress at plate center point E on the bottom surface. Figure 1.1 – Sketch representing the structure. Analysis Summary: Dim. Type Load Material Geometry Contact Solver Solution Method 3D Static Pressure Linear Linear - Implicit 1-Linear Units: Dimensional Data: = 1.0 , = 0.01 Material Data: Mass Density Young's Modulus Poisson's Ratio ρ= = ν = 11 × 7.80 10 × 2.07 10 0.3 /kg m Pa Load: Pressure Element Types: = × 7.0 10 Pa Belytschko-Tsay shell (elform=2) S/R Hughes-Liu shell (elform=6) Fully integrated shell (elform=16) Material Models: *MAT_001 or *MAT_ELASTIC Results Comparison: LS-DYNA maximum principal stress at plate center Point E (Node 13) on bottom surface ZU , are compared with Standard NAFEMS Benchmarks, Test plus its Z-displacement, LE6. Reference Condition - Point E (Node 13) Max Principal Stress (Pa) ZU (m) NAFEMS Benchmark Test LE6 0.802 10× - Belytschko-Tsay shell (elform=2) 0.781 10× 1.616 10− × − S/R Hughes-Liu shell (elform=6) 0.715 10× 1.507 10− × − Fully integrated shell (elform=16) 0.696 10× 1.404 10− × − These nodal displacement results were generated by *DATABASE_NODOUT keyword while the maximum principal stress results were generated by *DATABASE_ ELOUT. LS-DYNA stress and strain output corresponds to integration point locations. Stress at a node is an artifact of the post-processor and represents an average of the surrounding integration point stresses (the value will likely be different with different post- processors). Lobatto integration (intgrd=1 - *CONTROL_SHELL) was employed since it has an advantage in that the inner and outer integration points are on the shell surfaces. Gauss integration is the default through thickness integration rule (the default number of through thickness integration points is nip=2 - *SECTION_SHELL) in LS-DYNA, where 1-10 integration points may be specified, whereas, with Lobatto integration, 3-10 integration points may be specified (for 2 point integration, the Lobatto rule is very inaccurate). For this coarse meshing, the one-point quadrature (low order) Belytschko-Tsay shell (elform=2) provides a good stress comparison (Figure 1.2). The higher order, selectively reduced integration Hughes-Liu shell (elform=6) and the fully integrated Belytschko-Tsay shell (elform=16), which uses a 2x2 in-plane quadrature, provide comparatively stiffer results (Figure 1.3 and 1.4), probably due to the coarse meshing. Figure 1.3 – Element formulation 6 (S/R Hughes-Liu). *TITLE Skew Plate with Normal Pressure (thin shell mesh) *CONTROL_IMPLICIT_GENERAL $# imflag dt0 imform nsbs igs cnstn form 1 0.0 2 1 2 *CONTROL_IMPLICIT_SOLUTION $# nsolvr ilimit maxref dctol ectol rctol lstol abstol 1 11 15 0.001000 0.010000 0.0 0.900000 1.000000 $# dnorm diverg istif nlprint 2 1 1 2 $# arcctl arcdir arclen arcmth arcdmp 0 1 0.0 1 2 *CONTROL_SHELL $# wrpang esort irnxx istupd theory bwc miter proj 20.00000 0 0 0 2 2 1 $# rotascl intgrd lamsht cstyp6 tshell nfail1 nfail4 0.0 1 *CONTROL_TERMINATION $# endtim endcyc dtmin endeng endmas 1.000000 0 0.0 0.0 0.0 *DATABASE_ELOUT $# .....dt 1.0E-01 *DATABASE_BINARY_D3PLOT $# dt/cycl 0.100000 *DATABASE_HISTORY_SHELL $# eid1 eid2 eid3 eid4 ei5 eid6 eid7 eid8 6 7 10 11 *DEFINE_CURVE $# lcid sdir sfa sfo offa offo dattyp 1 0 0.0 0.0 0.0 0.0 $# a1 o1 0.0 0.0 1.00000000 700.0000000 *ELEMENT_SHELL $# eid pid n1 n2 n3 n4 n5 n6 n7 n8 1 1 1 6 7 2 16 1 19 24 25 20 *NODE $# nid x y z tc rc 1 0.0 0.0 0.0 3 25 1.86602540 0.50000000 0.0 3 *PART $# title material type # 1 (Elastic) $# pid secid mid eosid hgid grav adpopt tmid 1 1 1 *SECTION_SHELL $# secid elform shrf nip propt qr/irid icomp setyp 1 2 0.0 5 0 0.0 $ 1 6 0.0 5 0 0.0 $ 1 16 0.0 5 0 0.0 $# t1 t2 t3 t4 nloc marea 0.010000 0.010000 0.010000 0.010000 0 0.0 *MAT_ELASTIC $# mid ro e pr da db not used 1 7800.0002.1000e+11 0.300000 0.0 0.0 0.0 *LOAD_SEGMENT $# lcid sf at n1 n2 n3 n4 1 1.000000 0.0 1 6 7 2 1 1.000000 0.0 2 7 8 3 1 1.000000 0.0 3 8 9 4 1 1.000000 0.0 4 9 10 5 1 1.000000 0.0 7 12 13 8 1 1.000000 0.0 8 13 14 9 1 1.000000 0.0 9 14 15 10 1 1.000000 0.0 11 16 17 12 1 1.000000 0.0 12 17 18 13 1 1.000000 0.0 13 18 19 14 1 1.000000 0.0 14 19 20 15 1 1.000000 0.0 16 21 22 17 1 1.000000 0.0 17 22 23 18 1 1.000000 0.0 18 23 24 19 1 1.000000 0.0 19 24 25 20 *END 2. Skew Plate with Normal Pressure (thick shell mesh) Keywords: *CONTROL_IMPLICIT_GENERAL *CONTROL_IMPLICIT_SOLUTION Description: A skew plate of equal side lengths L and thickness t is subjected to a normal pressure P on the top face (Figure 2.1). The plate is meshed with thick shell elements with a 4 x 4 ZU = . density. The plate is simply supported on four side faces of the bottom surface, Determine the maximum principal stress at plate center point E on the bottom surface. Figure 2.1 – Sketch representing the structure. Analysis Summary: Dim. Type Load Material Geometry Contact Solver Solution Method 3D Static Pressure Linear Linear - Implicit 1-Linear Units: Dimensional Data: = 1.0 , = 0.01 Material Data: Mass Density Young's Modulus Poisson's Ratio ρ= = ν = 11 × 7.80 10 × 2.07 10 0.3 /kg m Pa Load: Pressure Element Types: = × 7.0 10 Pa S/R 2x2 IPI thick shell (elform=2) Assumed strain 2x2 IPI thick shell (elform=3) Assumed strain RI thick shell (elform=5) Material Models: *MAT_001 or *MAT_ELASTIC Results Comparison: LS-DYNA maximum principal stress at plate center Point E (Node 113) on bottom ZU , are compared with Standard NAFEMS Benchmarks, surface plus its Z-displacement, Test LE6. Reference Condition - Point E (Node113) Max Principal Stress (Pa) ZU (m) NAFEMS Benchmark Test LE6 0.802 10× - S/R 2x2 IPI thick shell (elform=2) 0.709 10× 1.496 10− × − Assumed strain 2x2 IPI thick shell (elform=3) 0.021 10× est. 0.084 10− × − Assumed strain RI thick shell (elform=5) 0.211 10× 0.849 10− × − These nodal displacement results were generated by *DATABASE_NODOUT keyword while results were generated by *DATABASE_ELOUT. the maximum principal (nodal) stress At least two elements through the thickness are usually recommended to capture bending response for assumed strain 2x2 IPI thick shell (elform=3) and assumed strain RI thick shell (elform=5) formulations. LS-DYNA stress and strain output corresponds to integration point locations. Stress at a node is an artifact of the post-processor and represents an average of the surrounding integration point stresses (the value will likely be different with different post- processors). Lobatto integration (intgrd=1 - *CONTROL_SHELL) was employed since it has an advantage in that the inner and outer integration points are on the shell surfaces. Gauss integration is the default through thickness integration rule (the default number of through thickness integration points is nip=2 - *SECTION_TSHELL) in LS-DYNA, where 1-10 integration points may be specified, whereas, with Lobatto integration, 3-10 integration points may be specified (for 2 point integration, the Lobatto rule is very inaccurate). Only the higher order selectively reduced 2x2 IPI thick shell (elform=2) provides a reasonable stress comparison (Figure 2.2). As with other higher order options, this formulation provides a comparatively stiff result, again probably due to the coarse meshing. The higher order assumed strain 2x2 IPI thick shell (elform=3) and assumed strain RI thick shell (elform=5) formulations do not provide acceptable solutions (Figure 2.3 and 2.4) since at least two elements through the thickness are usually recommended to Figure 2.2 – Element formulation 2 (S/R 2x2 IPI). Figure 2.4 - Element formulation 5 (assumed strain RI). Input Deck: *KEYWORD *TITLE Skew Plate with Normal Pressure (thick shell) *CONTROL_IMPLICIT_GENERAL $# imflag dt0 imform nsbs igs cnstn form 1 0.0 2 1 2 *CONTROL_IMPLICIT_SOLUTION $# nsolvr ilimit maxref dctol ectol rctol lstol abstol 1 11 15 0.001000 0.010000 0.0 0.900000 1.000000 $# dnorm diverg istif nlprint 2 1 1 2 $# arcctl arcdir arclen arcmth arcdmp 0 1 0.0 1 2 *CONTROL_SHELL $# wrpang esort irnxx istupd theory bwc miter proj 20.00000 0 0 0 2 2 1 $# rotascl intgrd lamsht cstyp6 tshell nfail1 nfail4 0.0 1 *CONTROL_TERMINATION $# endtim endcyc dtmin endeng endmas 1.000000 0 0.0 0.0 0.0 *DATABASE_ELOUT $# dt/cycl 1.0E-01 *DATABASE_BINARY_D3PLOT $# dt/cycl 0.100000 *DATABASE_HISTORY_TSHELL $# eid1 eid2 eid3 eid4 ei5 eid6 eid7 eid8 6 7 10 11 $# lcid sdir sfa sfo offa offo dattyp 1 0 0.0 0.0 0.0 0.0 $# a1 o1 0.0 0.0 1.00000000 700.0000000 *ELEMENT_TSHELL $# eid pid n1 n2 n3 n4 n5 n6 n7 n8 1 1 1 6 7 2 101 106 107 102 16 1 19 24 25 20 119 124 125 120 *NODE $# nid x y z tc rc 1 0.0 0.0 0.0 3 125 1.86602540 0.50000000 0.010 *PART $# title material type # 1 (Elastic) $# pid secid mid eosid hgid grav adpopt tmid 1 1 1 *SECTION_TSHELL $# secid elform shrf nip propt qr/irid icomp tshear 1 2 0.0 5 0 0.0 $ 1 3 0.0 5 0 0.0 $ 1 5 0.0 5 0 0.0 *MAT_ELASTIC $# mid ro e pr da db not used 1 7800.0002.1000e+11 0.300000 0.0 0.0 0.0 *LOAD_SEGMENT $# lcid sf at n1 n2 n3 n4 1 1.000000 0.0 101 106 107 102 1 1.000000 0.0 102 107 108 103 1 1.000000 0.0 103 108 109 104 1 1.000000 0.0 104 109 110 105 1 1.000000 0.0 106 111 112 107 1 1.000000 0.0 107 112 113 108 1 1.000000 0.0 108 113 114 109 1 1.000000 0.0 109 114 115 110 1 1.000000 0.0 111 116 117 112 1 1.000000 0.0 112 117 118 113 1 1.000000 0.0 113 118 119 114 1 1.000000 0.0 114 119 120 115 1 1.000000 0.0 116 121 122 117 1 1.000000 0.0 117 122 123 118 1 1.000000 0.0 118 123 124 119 1 1.000000 0.0 119 124 125 120 *END 3. Elliptical Thick Plate under Normal Pressure (coarse mesh) Keywords: *CONTROL_IMPLICIT_GENERAL *CONTROL_IMPLICIT_SOLUTION *CONTROL_IMPLICIT_SOLVER Description: An elliptical thick plate with thickness t is subjected to a normal pressure P on its top surface (Figure 3.1). The plate is meshed with solid hexahedra element with a 4 x 6 x 4 YU = ; face ABB′A′ has no X- density. Face CC′D′D has no Y-direction displacement, XU = ; the X and Y displacements of face BCC′B′ are fixed, = ; and the mid-plane (face BCC'B') has no X-, Y-, and Z-direction = . Determine the direct stress along Y-direction at point direction displacement, U= = = displacement, D. Analysis Summary: Dim. Type Load Material Geometry Contact Solver Solution Method 3D Static Pressure Linear Linear - Implicit 1-Linear Units: kg, m, s, N, Pa, N-m (kilogram, meter, second, Newton, Pascal, Newton-meter) Dimensional Data: = 1.0 , = 2.0 , = 1.75 , = 1.25 , = 0.60 Material Data: Mass Density Young's Modulus Poisson's Ratio ρ= = ν = 11 × 7.80 10 × 2.07 10 0.3 /kg m Pa Load: Pressure Element Types: = × 1.0 10 Pa Constant stress solid (elform=1) Fully integrated S/R solid (elform=2) Fully integrated S/R solid - for poor aspect ratio (eff) - (elform=-1) 8 point enhanced strain solid (elform=18) Material Models: *MAT_001 or *MAT_ELASTIC Results Comparison: LS-DYNA Y-direction stress at plate edge Point D (Node 29) on top surface plus its Z- ZU , are compared with NAFEMS Background to Benchmarks, Test LE10. Reference Condition - Point D (Node 29) Axial Stress σyy (Pa) ZU (m) NAFEMS Benchmark Test LE10 − × 5.38 10 - Constant stress solid (elform=1) − × 4.78 10 est 1.022 10− × − Fully integrated S/R solid (elform=2) − × 4.13 10 0.802 10− × − Fully integrated S/R solid (elform=-1) − × 5.35 10 1.005 10− × − 8 point enhanced strain solid (elform=18) − × 6.40 10 0.973 10− × − Estimated/extrapolated result calculated from − 3.67 10 Pa × centroid value. These nodal displacement results were generated by *DATABASE_NODOUT keyword while the axial stress (nodal) results were generated by *DATABASE_ELOUT (elout file) and *DATABASE_EXTENT_BINARY (eloutdet file provides detailed element output at integration points and connectivity nodes) keyword entries. You can set intout=stress or intout= all (*DATABASE_EXTENT_BINARY) and have stresses output file called eloutdet integration points (*DATABASE_ELOUT governs the output interval and *DATABASE_HISTORY_ SOLID governs which elements are output). Setting nodout=stress or nodout=all in *DATABASE_EXTENT_BINARY will write the extrapolated nodal stresses to eloutdet. for all to a the LS-DYNA stress and strain output corresponds to integration point locations. Stress at a node is an artifact of the post-processor and represents an average of the surrounding integration point stresses (the value will likely be different with different post- processors). For this coarse mesh, the one-point quadrature (low order) constant stress solid (elform=1) element formulation (the LS-DYNA default) provides a fair stress comparison (Figure 3.2). Refinement of the mesh should provide a better comparison. The higher order, fully integrated selectively reduced solid (elform=2), provides a comparatively stiff result (Figure 3.3), probably due to the coarse meshing. The aspect ratio of the elements varies throughout the coarse meshing. An available choice) intended to address poor aspect ratios (elform=-1). This formulation provides a good comparison for this coarse meshing (Figure 3.4). The 8 point enhanced strain solid (elform=18), developed for linear statics only, over predicts the stress (Figure 3.5); no explanation is currently available. Figure 3.3 – Element formulation 2 (fully integrated S/R). Figure 3.5 – Element formulation 18 (8 point enhanced strain). Input Deck: *KEYWORD *TITLE Elliptical Thick Plate under Normal Pressure (coarse mesh) *CONTROL_IMPLICIT_GENERAL $# imflag dt0 imform nsbs igs cnstn form 1 0.100000 2 1 2 *CONTROL_IMPLICIT_SOLUTION $# nsolvr ilimit maxref dctol ectol rctol lstol abstol 1 11 15 0.001000 0.010000 1.00e+10 0.900000 1.00e-10 *CONTROL_IMPLICIT_SOLVER $# lsolvr lprint negev order drcm drcprm autospc autotol 4 2 2 0 1 0.0 1 0.0 $# lcpack 2 *CONTROL_TERMINATION $# endtim endcyc dtmin endeng endmas 1.000000 0 0.0 0.0 0.0 *DATABASE_ELOUT $# dt binary lcur ioopt 1.0000E-9 0 0 *DATABASE_BINARY_D3PLOT $# dt/cycl 1.000000 *DATABASE_EXTENT_BINARY $# neiph neips maxint strflg sigflg epsflg rtflg engflg $# cmpflg ieverp beamip dcomp shge stssz n3thdt ialemat $# nintsld pkp_sen sclp hydro msscl therm intout nodout 8 1.0 stress stress *DATABASE_HISTORY_SOLID $# lcid sdir sfa sfo offa offo dattyp 1 0 0.0 0.0 0.0 0.0 $# a1 o1 0.0 0.0 1.00000000 1.0000000e+06 *ELEMENT_SOLID $# eid pid n1 n2 n3 n4 n5 n6 n7 n8 1 1 1 10 13 4 2 11 14 5 96 1 168 172 174 170 169 173 175 171 *NODE $# nid x y z tc rc 1 2.00000000 0.0 0.0 2 175 0.0 2.75000000 0.60000002 4 *PART $# title material type # 1 (Elastic) $# pid secid mid eosid hgid grav adpopt tmid 1 1 1 *SECTION_SOLID $# secid elform aet 1 1 1 $ 1 2 1 $ 1 -1 1 $ 1 18 1 *MAT_ELASTIC $# mid ro e pr da db not used 1 7800.0002.1000e+11 0.300000 0.0 0.0 0.0 *LOAD_SEGMENT $# lcid sf at n1 n2 n3 n4 1 1.000000 0.0 29 35 37 31 1 1.000000 0.0 31 37 39 33 1 1.000000 0.0 35 41 43 37 1 1.000000 0.0 37 43 45 39 1 1.000000 0.0 33 39 69 65 1 1.000000 0.0 65 69 71 67 1 1.000000 0.0 39 45 73 69 1 1.000000 0.0 69 73 75 71 1 1.000000 0.0 67 71 99 95 1 1.000000 0.0 95 99 101 97 1 1.000000 0.0 71 75 103 99 1 1.000000 0.0 99 103 105 101 1 1.000000 0.0 41 125 127 43 1 1.000000 0.0 43 127 129 45 1 1.000000 0.0 125 131 133 127 1 1.000000 0.0 127 133 135 129 1 1.000000 0.0 45 129 149 73 1 1.000000 0.0 73 149 151 75 1 1.000000 0.0 129 135 153 149 1 1.000000 0.0 149 153 155 151 1 1.000000 0.0 75 151 169 103 1 1.000000 0.0 103 169 171 105 1 1.000000 0.0 151 155 173 169 1 1.000000 0.0 169 173 175 171 *END Notes: 1. One should remember that the constant stress solid (elform=1), the fully integrated S/R solid (elform=2), and the fully integrated S/R solid (the so-called efficient formulation choice) intended to address poor aspect ratios (elform=-1) were originally 4. Elliptic Thick Plate under Normal Pressure (fine mesh) Keywords: *CONTROL_IMPLICIT_GENERAL *CONTROL_IMPLICIT_SOLUTION *CONTROL_IMPLICIT_SOLVER Description: An elliptical thick plate with thickness t is subjected to a normal pressure P on its top surface (Figure 4.1). The plate is meshed with solid hexahedra element with an 8 x 12 x YU = ; face ABB′A′ has no 4 density. Face CC′D′D has no Y-direction displacement, XU = ; the X and Y displacements of face BCC′B′ are fixed, = ; and the mid-plane (face BCC'B') has no X-, Y-, and Z-direction = . Determine the direct stress along Y-direction at point X-direction displacement, U= = = displacement, D. Analysis Summary: Dim. Type Load Material Geometry Contact Solver Solution Method 3D Static Pressure Linear Linear - Implicit 1-Linear Units: kg, m, s, N, Pa, N-m (kilogram, meter, second, Newton, Pascal, Newton-meter) Dimensional Data: = 1.0 , = 2.0 , = 1.75 , = 1.25 , = 0.60 Material Data: Mass Density Young's Modulus Poisson's Ratio ρ= = ν = 11 × 7.80 10 × 2.07 10 0.3 /kg m Pa Load: Pressure Element Types: = × 1.0 10 Pa Constant stress solid (elform=1) Fully integrated S/R solid (elform=2) Fully integrated S/R solid (elform=-1) 8 point enhanced strain solid (elform=18) Material Models: *MAT_001 or *MAT_ELASTIC Results Comparison: LS-DYNA Y-direction stress at plate edge Point D (Node 77) on top surface plus its Z- ZU , are compared with NAFEMS Background to Benchmarks, Test LE10. Reference Condition - Point D (Node 77) Axial Stress σyy (Pa) ZU (m) NAFEMS Benchmark Test LE10 − × 5.38 10 - Constant stress solid (elform=1) − × 5.30 10 est 1.051 10− × − Fully integrated S/R solid (elform=2) − × 4.70 10 0.947 10− × − Fully integrated S/R solid (elform=-1) − × 4.76 10 0.991 10− × − 8 point enhanced strain solid (elform=18) − × 6.28 10 0.982 10− × − Estimated/extrapolated result calculated from − 4.07 10 Pa × centroid value. These nodal displacement results were generated by *DATABASE_NODOUT keyword while the axial stress (nodal) results were generated by *DATABASE_ELOUT (elout file) and *DATABASE_EXTENT_BINARY (eloutdet file provides detailed element output at integration points and connectivity nodes) keyword entries. You can set intout=stress or intout=all (*DATABASE_EXTENT_BINARY) and have stresses output file called eloutdet integration points (*DATABASE_ELOUT governs the output interval and *DATABASE_HISTORY_ SOLID governs which elements are output). Setting nodout=stress or nodout=all in *DATABASE_EXTENT_BINARY will write the extrapolated nodal stresses to eloutdet. for all to a the LS-DYNA stress and strain output corresponds to integration point locations. Stress at a node is an artifact of the post-processor and represents an average of the surrounding integration point stresses (the value will likely be different with different post- processors). For this fine mesh, the one-point quadrature (low order) constant stress solid (elform=1) element formulation (the LS-DYNA default) provides a better stress comparison (Figure 4.2), when compared to the coarse mesh. The higher order, fully integrated selectively reduced solid (elform=2) still provides a comparatively stiff result (Figure 4.3); however, much improved over the coarse mesh. Doubling the elements in the x-y plane (mesh refinement) appears to have minimized the (the so-called efficient formulation choice) intended to address poor aspect ratios (elform=-1) now provides a very similar result (Figure 4.4) to the fully integrated S/R solid (elform=2). The 8 point enhanced strain solid (elform=18), developed for linear statics only, over predicts the stress result (Figure 4.5) by a fair amount (even with the change in mesh refinement); no explanation is presently available. Figure 4.3 – Element formulation 2 (fully integrated S/R). Figure 4.5 – Element formulation 18 (8 point enhanced strain). Input Deck: *KEYWORD *TITLE Thick Elliptic Plate under Normal Pressure (fine mesh) *CONTROL_IMPLICIT_GENERAL $# imflag dt0 imform nsbs igs cnstn form 1 0.100000 2 0 2 *CONTROL_IMPLICIT_SOLUTION $# nsolvr ilimit maxref dctol ectol rctol lstol abstol 1 11 15 0.001000 0.010000 1.00e+10 0.900000 1.00e-10 *CONTROL_IMPLICIT_SOLVER $# lsolvr lprint negev order drcm drcprm autospc autotol 4 2 2 0 0 0.0 0 0.0 $# lcpack 2 *CONTROL_TERMINATION $# endtim endcyc dtmin endeng endmas 1.000000 0 0.0 0.0 0.0 *DATABASE_ELOUT $# dt binary lcur ioopt 1.0000E-9 0 0 *DATABASE_BINARY_D3PLOT $# dt/cycl 1.000000 *DATABASE_EXTENT_BINARY $# neiph neips maxint strflg sigflg epsflg rtflg engflg $# cmpflg ieverp beamip dcomp shge stssz n3thdt ialemat $# nintsld pkp_sen sclp hydro msscl therm intout nodout 8 1.0 stress stress *DATABASE_HISTORY_SOLID $# id1 id2 id3 id4 id5 id6 id7 id8 1 0 0.0 0.0 0.0 0.0 $# a1 o1 0.0 0.0 1.00000000 1.0000000e+06 *ELEMENT_SOLID $# eid pid n1 n2 n3 n4 n5 n6 n7 n8 1 1 1 16 19 4 2 17 20 5 384 1 574 582 584 576 575 583 585 577 *NODE $# nid x y z tc rc 1 2.00000000 0.0 0.0 2 585 0.0 2.75000000 0.60000002 4 *PART $# title material type # 1 (Elastic) $# pid secid mid eosid hgid grav adpopt tmid 1 1 1 *SECTION_SOLID $# secid elform aet 1 1 1 $ 1 2 1 $ 1 -1 1 $ 1 18 1 *MAT_ELASTIC $# mid ro e pr da db not used 1 7800.000 2.100e+11 0.300000 0.0 0.0 0.0 *LOAD_SEGMENT $# lcid sf at n1 n2 n3 n4 1 1.000000 0.0 77 87 89 79 1 1.000000 0.0 79 89 91 81 1 1.000000 0.0 575 583 585 577 1 1.000000 0.0 575 583 585 577 *END Notes: 1. One should remember that the constant stress solid (elform=1), the fully integrated S/R solid (elform=2), and the fully integrated S/R solid (the so-called efficient formulation choice) intended to address poor aspect ratios (elform=-1) were originally 5. Snap-Back under Displacement Control Keywords: *CONTROL_IMPLICIT_AUTO *CONTROL_IMPLICIT_GENERAL *CONTROL_IMPLICIT_SOLUTION Description: In this problem the implicit arc length method is used in order to solve the snap-back of the system. With traditional Newton-based methods it is not possible to fully solve this problem, due to the null tangent stiffness matrix at a certain point of the analysis. Three DOF are present. A sketch representing the structure is shown below (Figure 5.1) along with a finite element representation (Figure 5.2). Figure 5.2 – The finite element representation of the problem. Four beams are used; the springs are modeled with discrete formulation, the truss is modeled with truss formulation. To avoid element inversion, the beams the springs are very long. Analysis Summary: Dim. Type Load Material Geometry Contact Solver 3D Static Force Linear Nonlinear - Implicit Solution Method 6–Arc length w/BFGS Units: non-dimensional Dimensional Data: L = × 2.50 10 , = × 1.00 10 − , Lα = × 2.50 10 Material Data: AE = × 5.0 10 , 1 =K 5.1 , = AE L / (1 + ) 1.9999 10 × = , 3 =K 25.0 , 4 =K 0.1 Load: Axial Load (load values of 0.6499 10 , 1.300 10 , 1.949 10 , 2.599 10 , 3.243 10 , 1.099 10 ) × − × × × × 0.0 varied linearly to 4.0 10 × P = Element Types: Truss (resultant) (elform=3) Discrete beam/cable (elform=6) Material Models: *MAT_001 or *MAT_ELASTIC *MAT_074 or *MAT_ELASTIC_SPRING_DISCRETE_BEAM Results Comparison: LS-DYNA displacements 3) are compared with NAFEMS Non-Linear Benchmarks, Test NL4 for each load value. BU , CV at locations A (Node 1), B (Node 2), and C (Node AU , NAFEMS NL4 LS-DYNA NAFEMS NL4 LS-DYNA NAFEMS NL4 LS-DYNA P (load) AU (disp) AU (disp) BU (disp) BU (disp) CV (disp) CV (disp) 0.6499 10× 650.0 650.0 0.0904 0.0903 5.241 5.242 1.300 10× 1300.0 1300.0 0.2328 0.2329 13.260 13.266 1.949 10× 1950.0 1949.0 0.5149 0.5150 27.080 27.079 2.599 10× 2600.0 2600.0 1.3440 1.3338 56.500 56.500 3.243 10× 3250.0 3250.0 7.0890 7.1053 162.600 162.850 -1.099 10× 3900.0 2800.0 4999.0 3898.500 41.950 2047.200 Figure 5.3 shows the displaced geometry at selected load values. These nodal displacement results (table above and Figures 5.4 and 5.5 below) were generated by *DATABASE_NODOUT keyword while the element stress results (Figures Figure 5.3 – Displaced geometry at selected loads. Figure 5.5 – Y-displacement vs. applied load for Node 3. Figure 5.7 – Axial force resultant vs. applied load for Elements 1 and 4. Input deck: *KEYWORD *TITLE Snap-Back Under Displacement Control *CONTROL_IMPLICIT_AUTO $# iauto iteopt itewin dtmin dtmax 1 20 5 1.000e-09 0.00100 *CONTROL_IMPLICIT_GENERAL $# imflag dt0 imform nsbs igs cnstn form 1 0.001000 2 1 2 1 *CONTROL_IMPLICIT_SOLUTION $# nsolvr ilimit maxref dctol ectol rctol lstol abstol 6 40 15 0.00100 0.01000 0.01000 0.900000 1.000000 $# dnorm diverg istif nlprint 2 1 1 2 $# arcctl arcdir arclen arcmth arcdmp 0 1 0.0 1 2 *CONTROL_TERMINATION $# endtim endcyc dtmin endeng endmas 1.000000 0 0.0 0.0 0.0 *DATABASE_ELOUT $# dt binary 1.0000e-04 1 *DATABASE_GLSTAT $# dt binary 1.0000e-04 1 *DATABASE_MATSUM $# dt binary 1.0000e-04 1 *DATABASE_NODFOR $# dt binary 1.0000e-04 1 *DATABASE_NODOUT $# dt binary 1.0000e-04 1 *DATABASE_BINARY_D3PLOT $# dt/cycl lcdt/nr beam npltc psetid 0.010000 *DATABASE_NODAL_FORCE_GROUP $# nsid cid 1 *DATABASE_HISTORY_BEAM $# eid1 eid2 eid3 eid4 ei5 eid6 eid7 eid8 1 2 3 4 *DATABASE_HISTORY_NODE $# nid1 nid2 nid3 nid4 ni5 nid6 nid7 nid8 1 2 3 4 5 *DEFINE_CURVE $# lcid sdir sfa sfo offa offo dattyp 1 0 0.0 0.0 0.0 0.0 $# a1 o1 0.0 0.0 1.00000000 4000.000000 *ELEMENT_BEAM $# eid pid n1 n2 n3 n4 n5 n6 n7 n8 1 1 5 3 0 0 0 0 0 2 2 2 3 2 0 0 0 0 0 2 3 3 2 4 0 0 0 0 0 2 4 4 2 1 0 0 0 0 0 2 *NODE $# nid x y z tc rc 1 -1.0000000e+04 0.0 0.0 2 0.0 0.0 0.0 3 2500.000000 25.00000000 0.0 4 6000.000000 0.0 0.0 5 2500.000000 3000.000000 0.0 *BOUNDARY_SPC_NODE $#nid/nsid cid dofx dofy dofz dofrx dofry dofrz 1 0 0 1 1 1 1 1 *BOUNDARY_SPC_NODE $#nid/nsid cid dofx dofy dofz dofrx dofry dofrz 2 0 0 1 1 1 1 1 3 0 1 0 1 1 1 1 4 0 1 1 1 1 1 1 5 0 1 1 1 1 1 1 *PART $# title Spring 1 $# pid secid mid eosid hgid grav adpopt tmid 1 1 1 *SECTION_BEAM $# secid elform shrf qr/irid cst scoor 1 6 1.000000 0 0 0.0 $# vol iner cid ca offset rrcon srcon trcon 1.000000 1.000000 0 0.0 0.0 0.0 0.0 0.0 *MAT_ELASTIC_SPRING_DISCRETE_BEAM $# mid ro k f0 d cdf tdf 1 1.000000 1.500000 0.0 0.0 0.0 0.0 $# flcid hlcid c1 c2 dle glcid 0 0 0.0 0.0 1.000000 *PART $# title Truss 2 $# pid secid mid eosid hgid grav adpopt tmid 2 2 2 *SECTION_BEAM $# secid elform shrf qr/irid cst scoor 2 3 0.0 0 0 0.0 $# a iss itt irr sa 1.000000 1.000000 1.000000 1.000000 1.000000 *MAT_ELASTIC $# title Spring 3 $# pid secid mid eosid hgid grav adpopt tmid 3 1 3 *MAT_ELASTIC_SPRING_DISCRETE_BEAM $# mid ro k f0 d cdf tdf 3 1.000000 0.250000 0.0 0.0 0.0 0.0 $# flcid hlcid c1 c2 dle glcid 0 0 0.0 0.0 1.000000 *PART $# title Spring 4 $# pid secid mid eosid hgid grav adpopt tmid 4 1 4 *MAT_ELASTIC_SPRING_DISCRETE_BEAM $# mid ro k f0 d cdf tdf 4 1.000000 1.000000 0.0 0.0 0.0 0.0 $# flcid hlcid c1 c2 dle glcid 0 0 0.0 0.0 1.000000 *LOAD_NODE_POINT $# node dof lcid sf cid m1 m2 m3 1 1 1 1.000000 *SET_NODE_LIST $# sid da1 da2 da3 da4 solver 1 0.0 0.0 0.0 0.0 $# nid1 nid2 nid3 nid4 nid5 nid6 nid7 nid8 1 2 3 4 5 *END Notes: 1. Using the default values (i.e., BFGS without arc length) and an automatic time stepping control, it was possible to solve the problem only up to a certain load. At this point, (a) the BFGS solution method cannot go any further, due to the tangent stiffness matrix becoming close to null, resulting in a FATAL ERROR – nonlinear solver failed to find equilibrium, or (b) the solution proceeded with an incorrect solution (no snap-back). 2. When the time step was allowed to increase up to 0.010, either by initial time step or dtmax (automatic time stepping control), a solution could be achieved, relatively quickly, but a somewhat noisy in the response. 3. Using the default tolerance (default=inactive) for the residual (force) norm appeared to result in non-convergence or inaccurate convergence (i.e. relative convergence was achieved, but the amount of out-of-balance forces became too large to guarantee the accuracy of the solution). The tolerance on force was therefore activated and set to (0.010). If this value is too large, convergence issues will result. 4. In addition to employing the BFGS solver with arc length (nsolvr=6), it was found necessary to employ the default arc length, that is, the generalized arc length method (arcctl=0), where the norm of the global displacement vector controls the solution; this includes all nodes. Attempts at employing the option whereby the arc length 6. Straight Cantilever Beam with Axial End Point Load Keywords: *CONTROL_IMPLICIT_AUTO *CONTROL_IMPLICIT_GENERAL *CONTROL_IMPLICIT_SOLVER *CONTROL_IMPLICIT_SOLUTION Description: The analysis involves a cantilever beam loaded at one end with a quasi-axial load (axial component=100 normal component). The material is elastic. The X-displacement, the Y-displacement and the Z-rotation of the end point of the beam are determined. A sketch representing the structure is shown below (Figure 6.1) along with the finite element model (Figure 6.2). Figure 6.2 – Finite element model with applied loads and boundary conditions. Analysis Summary: Dim. Type Load Material Geometry Contact Solver 3D Static Force Linear Nonlinear - Implicit Solution Method 2-Nonlinear w/BFGS Units: kg, m, s, N, Pa, N-m (kilogram, meter, second, Newton, Pascal, Newton-meter) Dimensional Data: The beam has a constant square section (0.1m x 0.1m) and a total length of 3.2 m and is meshed with 32 beams of equal length. Material Data: Mass Density Young's Modulus Poisson's Ratio ρ= = ν = 11 × 7.85 10 × 2.10 10 0.0 /kg m Load: Axial Load Pressure Element Types: = 3.844 10 × = 3.844 10 × Hughes-Liu beam with cross section integration (elform=1) Material Models: *MAT_001 or *MAT_ELASTIC Results Comparison: LS-DYNA displacements with NAFEMS Non-Linear Benchmarks, Test NL6. XU , YU , ZR at the end of the beam (Node 6) are compared XU (m) YU (m) ZR (rad) NAFEMS NL6 -5.0404 -1.3472 -3.0725 Node 6 -5.0629 -1.3607 -3.0646 These nodal displacement results were generated by *DATABASE_NODOUT keyword. ZR ) histories for Node The X-displacement ( 6 are given in Figure 6.3. Figures 6.4 and 6.5 provide the contour plot of the bending moment and the axial force, respectively, at the end of the step. XU ), Y-displacement ( Figure 6.3 – X-displacement, Y-displacement, and Z-rotation for Node 6. Figure 6.5 – Contour plot of the axial force at the end of the step. Input deck: *KEYWORD *TITLE Straight Cantilever with Axial End Point Load *CONTROL_IMPLICIT_AUTO $# iauto iteopt itewin dtmin dtmax 1 11 5 0.010000 *CONTROL_IMPLICIT_GENERAL $# imflag dt0 imform nsbs igs cnstn form 1 0.010000 2 0 2 *CONTROL_IMPLICIT_SOLVER $# lsolvr lprint negev order drcm drcprm autospc autotol 5 2 2 0 1 0.0 1 0.0 $# lcpack 2 *CONTROL_IMPLICIT_SOLUTION $# nsolvr ilimit maxref dctol ectol rctol lstol abstol 2 11 15 0.0010 0.0100 1.00e+10 0.900000 1.00e-10 $# dnorm diverg istif nlprint nlnorm 2 1 1 2 1 $# arcctl arcdir arclen arcmth arcdmp 6 1 0.0 1 2 *CONTROL_OUTPUT $# npopt neecho nrefup iaccop opifs ipnint ikedit iflush 1 3 1 0 0.0 0 1000 5000 $# iprtf 3 *CONTROL_TERMINATION $# endtim endcyc dtmin endeng endmas 1.000000 0 0.0 0.0 0.0 *DATABASE_NCFORC $# dt binary 0.001000 1 *DATABASE_NODOUT $# dt binary 0.001000 1 *DATABASE_NODAL_FORCE_GROUP $# nsid cid 2 *DATABASE_HISTORY_NODE $# nid1 nid2 nid3 nid4 ni5 nid6 nid7 nid8 6 *DATABASE_HISTORY_BEAM $# eid1 eid2 eid3 eid4 ei5 eid6 eid7 eid8 3 *DEFINE_CURVE $# lcid sdir sfa sfo offa offo dattyp 1 0 1.000000 1.000000 0.0 0.0 $# a1 o1 0.0 0.0 1.00000000 3.8440088e+06 *DEFINE_CURVE $# lcid sdir sfa sfo offa offo dattyp 2 0 1.000000 1.000000 0.0 0.0 $# a1 o1 0.0 0.0 1.00000000 38440.08545 *ELEMENT_BEAM $# eid pid n1 n2 n3 n4 n5 n6 n7 n8 1 1 1 2 3 0 0 0 0 2 33 1 2 92 97 0 0 0 0 2 *NODE $# nid x y z tc rc 1 0.0 0.0 0.0 97 0.15000001 0.0 0.01000000 *BOUNDARY_SPC_NODE $#nid/nsid cid dofx dofy dofz dofrx dofry dofrz 1 0 1 1 1 1 1 1 *PART $# title $# pid secid mid eosid hgid grav adpopt tmid 1 1 1 *SECTION_BEAM $# secid elform shrf qr/irid cst scoor 1 1 0.830000 2 0 0.0 $# ts1 ts2 tt1 tt2 nsloc ntloc 0.100000 0.100000 0.100000 0.100000 *MAT_ELASTIC $# mid ro e pr da db not used 1 7850.0002.1000e+11 0.0 0.0 0.0 0.0 *LOAD_NODE_POINT $# node dof lcid sf cid m1 m2 m3 6 1 1 -1.000000 *LOAD_NODE_POINT $# node dof lcid sf cid m1 m2 m3 6 2 2 -1.000000 *SET_NODE_LIST_GENERATE $# sid da1 da2 da3 da4 solver 1 0.0 0.0 0.0 0.0 $# nid1 nid2 nid3 nid4 nid5 nid6 nid7 nid8 2 92 *SET_NODE_LIST $# sid da1 da2 da3 da4 solver 2 0.0 0.0 0.0 0.0 $# nid1 nid2 nid3 nid4 nid5 nid6 nid7 nid8 6 Notes: 1. Using the default values, with an initial time step dt0=0.010, the problem stops at the 12th iteration due to an energy increase. The *CONTROL_IMPLICIT_GENERAL, *CONTROL_IMPLICIT_SOLUTION, and *CONTROL_IMPLICIT_SOLVER, with no automatic time stepping (*CONTROL_IMPLICIT_AUTO) are considered to be the default keywords. 2. Allowing more iterations (*CONTROL_IMPLICIT_SOLUTION) will not help to solve the problem. 3. To resolve the energy increase and termination stated above, include the automatic time stepping (*CONTROL_IMPLICIT_AUTO) entry, in particular the specification of dtmax. The following situations occur when using different values of dtmax: dtmax =blank (10*dt0) or 0.100 (these are actually the same); the current step size will increase right off, eventually two energy increases will occur, where time steps are then decreased, with the simulation then continuing until termination is reached. This takes the least iterations with ASCII result plots somewhat noisy. dtmax =0.010 (the initial time step); solves very nicely with no energy increases, takes about 50 percent more iterations than dtmax=0.100, with smoother ASCII result plots. dtmax =0.001 yielded the same results as dtmax =0.010. dt0 appeared to still be considered in the time step options. 4. It is also possible to achieve a successful solution specifying an initial time step of dt0=0.001 and a similar value for the maximum allowable time step (dtmax=0.001 in the *CONTROL_IMPLICIT_AUTO keyword). Using these parameters will increase 7. Lee’s Frame Buckling Problem Keywords: *CONTROL_IMPLICIT_AUTO *CONTROL_IMPLICIT_GENERAL *CONTROL_IMPLICIT_SOLUTION Description: The problem involves a framed structure deforming under the action of a load applied on one node. The frame is pinned to the ground at two nodes and the load is applied on Node 56, as shown in Figure 7-1. The finite element model is shown in Figure 7.2. The length of the two beams is 1.2 m. The height of the square cross section is 0.02 m and the thickness is 0.03 m. When a certain load is reached, the structure undergoes buckling and the load-deflection curve shows a typical snap-back behavior, shown in Figure 7-3. Arc-length method is required in order to capture the post-buckling behavior of the structure. Figure 7.2 – Finite element model with applied loads and boundary conditions. Analysis Summary: Dim. Type Load Material Geometry Contact Solver 3D Static Force Linear Nonlinear - Implicit Solution Method 6-Arc length w/BFGS Units: kg, m, s, N, Pa, N-m (kilogram, meter, second, Newton, Pascal, Newton-meter) Dimensional Data: The beam has a constant square section (0.1m x 0.1m) and a total length of 3.2 m and is Material Data: Mass Density Young's Modulus Poisson's Ratio ρ= = ν = Load: × 7.85 10 × 7.174 10 0.0 /kg m 10 Pa Load is applied incrementally to the structure until buckling occurs. Element Types: Hughes-Liu beam with cross section integration (elform=1) Material Models: *MAT_001 or *MAT_ELASTIC Results Comparison: LS-DYNA displacements the critical (buckling) load Test NL7. XU and YU , at the location of the applied load (Node 56), plus critP , are compared with NAFEMS Non-Linear Benchmarks, XU (m) NAFEMS NL7 - YU (m) 0.4884 Node 56 0.2620 0.4826 critP (N) 1.8485 10× 1.8228 10× These nodal displacement results were generated by *DATABASE_NODOUT keyword. From *DATABASE_NODOUT results, it was also seen that the critical load increment is at 0.364568 of the total load, which would therefore correspond to a load of . critP × 0.364568 5.0 10 1.8228 10 = × × = Figure 7.4 gives the X-displacement, Y-displacement, and resultant displacement versus Figure 7.3 – Displaced configuration at the buckling load. Figure 7.4 – X-displacement, Y-displacement, and resultant *TITLE Lee's Frame Buckling Problem *CONTROL_IMPLICIT_AUTO $# iauto iteopt itewin dtmin dtmax 1 20 5 1.000e-09 *CONTROL_IMPLICIT_GENERAL $# imflag dt0 imform nsbs igs cnstn form 1 0.003000 2 100 2 1 *CONTROL_IMPLICIT_SOLUTION $# nsolvr ilimit maxref dctol ectol rctol lstol abstol 6 30 15 1.000e-06 1.000e-05 1.000e-05 0.990000 1.000000 $# dnorm diverg istif nlprint 2 1 1 2 $# arcctl arcdir arclen arcmth arcdmp 0 1 0.0 1 2 *CONTROL_TERMINATION $# endtim endcyc dtmin endeng endmas 1.000000 0 0.0 0.0 0.0 *DATABASE_GLSTAT $# dt binary 0.001000 1 *DATABASE_MATSUM $# dt binary 0.001000 1 *DATABASE_NODFOR $# dt binary 1.0000e-04 1 *DATABASE_NODOUT $# dt binary 1.0000e-04 1 *DATABASE_BINARY_D3PLOT $# dt/cycl lcdt/nr beam npltc psetid 0.010000 0 2 *DATABASE_NODAL_FORCE_GROUP $# nsid cid 1 *DATABASE_HISTORY_NODE $# nid1 nid2 nid3 nid4 ni5 nid6 nid7 nid8 56 36 1 *DEFINE_CURVE $# lcid sdir sfa sfo offa offo dattyp 1 0 1.000000 1.000000 0.0 0.0 $# a1 o1 0.0 0.0 1.00000000 5.0000000e+04 *ELEMENT_BEAM $# eid pid n1 n2 n3 n4 n5 n6 n7 n8 1 1 1 2 3 0 0 0 0 2 31 1 32 56 61 0 0 0 0 2 *NODE $# nid x y z tc rc 1 0.0 0.0 0.0 61 0.17999999 1.20000005 0.10000000 *BOUNDARY_SPC_NODE $#nid/nsid cid dofx dofy dofz dofrx dofry dofrz 1 0 1 1 1 1 1 *BOUNDARY_SPC_NODE $#nid/nsid cid dofx dofy dofz dofrx dofry dofrz 36 0 1 1 1 1 1 *PART $# title $# pid secid mid eosid hgid grav adpopt tmid 1 1 1 $# secid elform shrf qr/irid cst scoor 1 1 0.830000 5 0 0.0 $# ts1 ts2 tt1 tt2 nsloc ntloc 0.030000 0.030000 0.02 0.02 *MAT_ELASTIC $# mid ro e pr da db not used 1 7850.0007.1740e+10 0.0 0.0 0.0 0.0 *LOAD_NODE_POINT $# node dof lcid sf cid m1 m2 m3 56 2 1 -1.000000 *SET_NODE_LIST $# sid da1 da2 da3 da4 solver 1 0.0 0.0 0.0 0.0 $# nid1 nid2 nid3 nid4 nid5 nid6 nid7 nid8 1 6 36 56 *END 8. Pin-Ended Double Cross: In-Plane Vibration Keywords: *CONTROL_IMPLICIT_AUTO *CONTROL_IMPLICIT_EIGENVALUE *CONTROL_IMPLICIT_GENERAL *CONTROL_IMPLICIT_SOLVER Description: This example shows the behavior of beam elements in a modal analysis. The structure is a double cross pinned to the ground as show in Figure 8.1. All inner nodes have = . On the outer nodes = . = = = = = = The finite element model is shown in Figure 8.2. The problem requires the extraction of numerically close eigenvalues, making it an ideal benchmark to check the element formulation accuracy. Each arm of the cross is modeled with 4 beams, for a total of 32 beams. The length of each arm is 5 m. Figure 8.2 – Finite element model with end point boundary conditions. Analysis Summary: Dim. Type Load Material Geometry Contact Solver 3D Modal - Linear Linear - Implicit Solution Method Block Shift and Inverted Lanczos Units: kg, m, s, N, Pa, N-m (kilogram, meter, second, Newton, Pascal, Newton-meter) Dimensional Data: Material Data: Mass Density Young's Modulus Poisson's Ratio ρ= = ν = Element Types: 11 × 8.00 10 × 2.00 10 0.3 /kg m Pa Hughes-Liu beam with cross section integration (elform=1) Belytschko-Schwer resultant beam (elform=2) Small displacement, linear Timoshenko beam with exact stiffness (elform=13) Material Models: *MAT_001 or *MAT_ELASTIC Results Comparison: LS-DYNA natural frequencies, first 16 (frequency in Hertz), and mode shapes (first 6) are compared with Standard NAFEMS Benchmarks, Test FV2. Mode(s) NAFEMS FV2 (Hz) Hughes-Liu Beam (Hz) Belytschko- Schwer Beam Timoshenko Beam (Hz) 1 2, 3 11.336 11.641 11.323 11.365 17.709 19.080 17.621 17.803 4, 5, 6, 7, 8 17.709 19.115 17.649 17.832 9 45.345 51.691 44.833 45.620 10, 11 57.390 73.717 55.673 57.399 12, 13, 14, 15, 16 57.390 74.381 55.952 As seen in the results, using the LS-DYNA default beam (Hughes-Liu - elform=1) results in poor accuracy in the frequency calculation due to its omission of the first (no bending) and second (no rotary inertia) order terms (more elements are often needed in an attempt to overcome this limitation). The Hughes-Liu beam effectively generates a constant moment along its length, so, as with brick and shell elements, meshes need to be reasonably fine to achieve adequate accuracy. The Belytschko-Schwer beam (elform=2) provides good frequency results throughout most of the range covered, with some minor differences at the higher frequency range. This element is often acceptable. The Timoshenko beam (elform=13), with its inclusion of second order (rotary inertia and shear distortion) terms, provides very good results throughout the reported frequency range. This element formulation is generally recommended for this type of frequency analysis. Eigenvalue Results: From the eigout file, generated by the *CONTROL_IMPLICIT_EIGENVALUE keyword: Hughes-Liu beam (elform=1): Pin-Ended Double Cross: In-Plane Vibration r e s u l t s o f e i g e n v a l u e a n a l y s i s: |------ frequency -----| MODE EIGENVALUE RADIANS CYCLES PERIOD 1 5.349990E+03 7.314363E+01 1.164117E+01 8.590202E-02 2 1.437182E+04 1.198825E+02 1.907989E+01 5.241119E-02 3 1.437182E+04 1.198825E+02 1.907989E+01 5.241119E-02 4 1.442423E+04 1.201009E+02 1.911465E+01 5.231589E-02 5 1.442423E+04 1.201009E+02 1.911465E+01 5.231589E-02 6 1.442423E+04 1.201009E+02 1.911465E+01 5.231589E-02 7 1.442423E+04 1.201009E+02 1.911465E+01 5.231589E-02 8 1.442423E+04 1.201009E+02 1.911465E+01 5.231589E-02 9 1.054860E+05 3.247862E+02 5.169132E+01 1.934561E-02 10 2.145341E+05 4.631783E+02 7.371711E+01 1.356537E-02 11 2.145341E+05 4.631783E+02 7.371711E+01 1.356537E-02 12 2.184158E+05 4.673498E+02 7.438102E+01 1.344429E-02 13 2.184158E+05 4.673498E+02 7.438102E+01 1.344429E-02 14 2.184158E+05 4.673498E+02 7.438102E+01 1.344429E-02 15 2.184158E+05 4.673498E+02 7.438102E+01 1.344429E-02 Belytschko-Schwer beam (elform=2): Pin-Ended Double Cross: In-Plane Vibration r e s u l t s o f e i g e n v a l u e a n a l y s i s: |------ frequency -----| MODE EIGENVALUE RADIANS CYCLES PERIOD 1 5.061497E+03 7.114420E+01 1.132295E+01 8.831620E-02 2 1.225757E+04 1.107139E+02 1.762066E+01 5.675155E-02 3 1.225757E+04 1.107139E+02 1.762066E+01 5.675155E-02 4 1.229691E+04 1.108915E+02 1.764892E+01 5.666068E-02 5 1.229691E+04 1.108915E+02 1.764892E+01 5.666068E-02 6 1.229691E+04 1.108915E+02 1.764892E+01 5.666068E-02 7 1.229691E+04 1.108915E+02 1.764892E+01 5.666068E-02 8 1.229691E+04 1.108915E+02 1.764892E+01 5.666068E-02 9 7.935148E+04 2.816939E+02 4.483298E+01 2.230501E-02 10 1.223614E+05 3.498019E+02 5.567270E+01 1.796212E-02 11 1.223614E+05 3.498019E+02 5.567270E+01 1.796212E-02 12 1.235904E+05 3.515543E+02 5.595161E+01 1.787259E-02 13 1.235904E+05 3.515543E+02 5.595161E+01 1.787259E-02 14 1.235904E+05 3.515543E+02 5.595161E+01 1.787259E-02 15 1.235904E+05 3.515543E+02 5.595161E+01 1.787259E-02 16 1.235904E+05 3.515543E+02 5.595161E+01 1.787259E-02 Timoshenko beam (elform=13): Pin-Ended Double Cross: In-Plane Vibration r e s u l t s o f e i g e n v a l u e a n a l y s i s: |------ frequency -----| MODE EIGENVALUE RADIANS CYCLES PERIOD 1 5.099519E+03 7.141092E+01 1.136540E+01 8.798634E-02 2 1.251262E+04 1.118598E+02 1.780305E+01 5.617016E-02 3 1.251262E+04 1.118598E+02 1.780305E+01 5.617016E-02 4 1.255348E+04 1.120423E+02 1.783209E+01 5.607869E-02 5 1.255348E+04 1.120423E+02 1.783209E+01 5.607869E-02 6 1.255348E+04 1.120423E+02 1.783209E+01 5.607869E-02 7 1.255348E+04 1.120423E+02 1.783209E+01 5.607869E-02 8 1.255348E+04 1.120423E+02 1.783209E+01 5.607869E-02 9 8.216358E+04 2.866419E+02 4.562048E+01 2.191998E-02 10 1.300676E+05 3.606489E+02 5.739905E+01 1.742189E-02 11 1.300676E+05 3.606489E+02 5.739905E+01 1.742189E-02 12 1.314649E+05 3.625808E+02 5.770653E+01 1.732906E-02 13 1.314649E+05 3.625808E+02 5.770653E+01 1.732906E-02 14 1.314649E+05 3.625808E+02 5.770653E+01 1.732906E-02 15 1.314649E+05 3.625808E+02 5.770653E+01 1.732906E-02 16 1.314649E+05 3.625808E+02 5.770653E+01 1.732906E-02 Mode Shapes (first six): From the d3plot file, generated by the *DATABASE_BINARY_D3PLOT keyword, the user can obtain the first six mode shapes (stick view) for the Hughes-Li beam (Figure 8.3), the Belytschko-Schwer Beam (Figure 8.4), and the Timoshenko beam (Figure 8.5). Displacement contouring of the first six mode shapes are given in Figures 8.6, 8.7, and Figure 8.3 - Mode shapes for Hughes-Liu beam (stick view). Figure 8.5 - Mode shapes for Timoshenko beam (stick view). Figure 8.7 - Mode shapes for Belytschko beam (displacement contouring). *TITLE Pin-Ended Double Cross: In-Plane Vibration *CONTROL_IMPLICIT_AUTO $# iauto iteopt itewin dtmin dtmax 1 11 15 0.0 0.0 *CONTROL_IMPLICIT_EIGENVALUE $# neig center lflag lftend rflag rhtend eigmth shfscl 16 11.000 0 -1.00e+29 0 1.00e+29 2 0.0 *CONTROL_IMPLICIT_GENERAL $# imflag dt0 imform nsbs igs cnstn form 1 1.00e-04 2 1 2 *CONTROL_IMPLICIT_SOLVER $# lsolvr lprint negev order drcm drcprm autospc autotol 16 1 1 0 1 0.0 1 0.0 *DATABASE_BINARY_D3PLOT $# dt/cycl lcdt/nr beam npltc psetid 0.010000 0 2 *ELEMENT_BEAM $# eid pid n1 n2 n3 n4 n5 n6 n7 n8 1 1 1 2 3 0 0 0 0 2 32 1 61 74 76 0 0 0 0 2 *NODE $# nid x y z tc rc 1 0.0 0.0 0.0 76 2.79029131 -2.20970869 1.00000000 *BOUNDARY_SPC_SET $#nid/nsid cid dofx dofy dofz dofrx dofry dofrz 2 0 1 1 1 1 1 0 *BOUNDARY_SPC_SET $#nid/nsid cid dofx dofy dofz dofrx dofry dofrz 1 0 0 0 1 1 1 0 *PART $# title $# pid secid mid eosid hgid grav adpopt tmid 1 1 1 *SECTION_BEAM $# secid elform shrf qr/irid cst scoor 1 1 0.833333 2.0 0.0 0.0 $# ts1 ts2 tt1 tt2 nsloc ntloc 0.125000 0.125000 0.125000 0.125000 0.0 0.0 $$# secid elform shrf qr/irid cst scoor $ 1 2 0.833333 2 0 0.0 $$# a iss itt j sa ist $ 0.01562502.0345e-052.0345e-054.0690e-050.01302083 $$# secid elform shrf qr/irid cst scoor $ 1 13 0.833333 2 0 0.0 $$# a iss itt j sa ist $ 0.01562502.0345e-052.0345e-054.0690e-050.01302083 *MAT_ELASTIC $# mid ro e pr da db not used 1 8000.0002.0000e+11 0.300000 0.0 0.0 0.0 *SET_NODE_LIST_GENERATE $# sid da1 da2 da3 da4 solver 1 0.0 0.0 0.0 0.0 $# b1beg b1end b2beg b2end b3beg b3end b4beg b4end 2 4 6 24 27 29 31 42 44 46 48 59 61 63 65 76 *SET_NODE_LIST $# sid da1 da2 da3 da4 solver 2 0.0 0.0 0.0 0.0 $# nid1 nid2 nid3 nid4 nid5 nid6 nid7 nid8 1 5 30 47 64 60 43 26 Notes: 1. The main difference among these element formulations is the inclusion of different second order terms for rotary inertia and shear distortion. The Euler (Belytschko- Schwer) beam model includes only the first order terms, lateral displacement and bending moment. The simple shear (Hughes-Liu) beam model includes only the translation first order term (no bending) plus shear distortion, while the Timoshenko beam model includes both rotary inertia and shear distortion in addition to the first 9. Simply Supported Thin Annular Plate (coarse mesh) Keyword: *CONTROL_IMPLICIT_EIGENVALUE *CONTROL_IMPLICIT_GENERAL Description: A simply-supported annular plate of thickness t=0.06 m is to be analyzed to determine the first nine natural frequencies. The inner radius is 1.8 m and the outer radius is 6.0 m. This coarse mesh analysis has 26 shell elements (circumferential) by 3 elements (radial). All nodes have = . On the outer nodes = = ZU = . A sketch representing the structure is shown below (Figure 9.1) along with the finite element model (Figure 9.2). Figure 9.2 – Coarse mesh finite element model with simply supported boundary conditions on outer nodes. Analysis Summary: Dim. Type Load Material Geometry Contact Solver 3D Modal - Linear Linear - Implicit Solution Method Block Shift and Inverted Lanczos Units: kg, m, s, N, Pa, N-m (kilogram, meter, second, Newton, Pascal, Newton-meter) Dimensional Data: ro 6= , ri 8.1= , 06.0= Material Data: Mass Density Young's Modulus Poisson's Ratio ρ= = ν = Element Types: 11 × 8.00 10 × 2.00 10 0.3 /kg m Pa Fully integrated shell (elform=16) Material Models: *MAT_001 or *MAT_ELASTIC Results Comparison: LS-DYNA natural frequencies, first 10 (frequency in Hertz), and mode shapes (first 5) are compared with NAFEMS Natural Frequency Benchmark NF14. Mode(s) NAFEMS NF14 (Hz) Coarse Mesh (Hz) 1 2, 3 4, 5 6 7, 8 9, 10 1.870 5.137 9.673 14.850 15.570 18.380 1.806 5.423 10.179 13.217 16.239 16.691 It is seen that even with this rather coarse mesh refinement, the LS-DYNA natural frequency results provide a fair comparison with the NAFEMS Selected Benchmarks for Eigenvalue Results: From the eigout file, generated by the *CONTROL_IMPLICIT_EIGENVALUE keyword: Simply Supported Thin Annular Plate (coarse mesh) r e s u l t s o f e i g e n v a l u e a n a l y s i s: |------ frequency -----| MODE EIGENVALUE RADIANS CYCLES PERIOD 1 1.287078E+02 1.134495E+01 1.805604E+00 5.538311E-01 2 1.161053E+03 3.407423E+01 5.423083E+00 1.843970E-01 3 1.161053E+03 3.407423E+01 5.423083E+00 1.843970E-01 4 4.090826E+03 6.395957E+01 1.017948E+01 9.823683E-02 5 4.090827E+03 6.395957E+01 1.017948E+01 9.823683E-02 6 6.896060E+03 8.304252E+01 1.321663E+01 7.566227E-02 7 1.041122E+04 1.020354E+02 1.623944E+01 6.157849E-02 8 1.041122E+04 1.020354E+02 1.623944E+01 6.157848E-02 9 1.099787E+04 1.048707E+02 1.669070E+01 5.991361E-02 10 1.099787E+04 1.048707E+02 1.669070E+01 5.991361E-02 Mode Shapes (first five): Figures 9.3, 9.4, and 9.5 show the first 5 mode shapes with no contouring while Figures 9.6. 9.7, and 9.8 show the same 5 mode shapes with displacement contouring. Figure 9.4 - Modes 2 and 3, 5.423 Hz (NAFEMS 5.137) - no contouring. Figure 9.6 - Mode 1, 1.806 Hz (NAFEMS 1.870) - displacement contouring. Figure 9.8 - Modes 4 and 5, 10.179 Hz (NAFEMS 9.673) - displacement contouring. 64 *TITLE Simply Supported Thin Annular Plate (coarse mesh) *CONTROL_IMPLICIT_EIGENVALUE $# neig center lflag lftend rflag rhtend eigmth shfscl 10 0.0 1 1.000000 1 30.00000 2 0.0 *CONTROL_IMPLICIT_GENERAL $# imflag dt0 imform nsbs igs cnstn form 1 1.000000 *CONTROL_TERMINATION $# endtim endcyc dtmin endeng endmas 1.000000 0 0.0 0.0 0.0 *DATABASE_BINARY_D3PLOT $# dt/cycl lcdt/nr beam npltc psetid 1.000000 *ELEMENT_SHELL $# eid pid n1 n2 n3 n4 n5 n6 n7 n8 1 1 1 27 28 2 78 1 78 104 79 53 *NODE $# nid x y z tc rc 1 1.79999995 0.0 0.0 104 5.82565355 -1.43588233 0.0 3 1 *BOUNDARY_SPC_SET $#nid/nsid cid dofx dofy dofz dofrx dofry dofrz 1 0 1 1 1 0 0 1 *BOUNDARY_SPC_SET $#nid/nsid cid dofx dofy dofz dofrx dofry dofrz 2 0 1 1 0 0 0 1 *PART $# title material type # 1 (Elastic) $# pid secid mid eosid hgid grav adpopt tmid 1 1 1 *SECTION_SHELL $# secid elform shrf nip propt qr/irid icomp setyp 1 16 0.0 0 1 0.0 0 1 $# t1 t2 t3 t4 nloc marea 0.060000 0.060000 0.060000 0.060000 0 0.0 *MAT_ELASTIC $# mid ro e pr da db not used 1 8000.0002.0000e+11 0.300000 0.0 0.0 0.0 *SET_NODE_LIST_GENERATE $# sid da1 da2 da3 da4 solver 1 0.0 0.0 0.0 0.0 $# b1beg b1end b2beg b2end b3beg b3end b4beg b4end 79 104 *SET_NODE_LIST_GENERATE $# sid da1 da2 da3 da4 solver 2 0.0 0.0 0.0 0.0 $# b1beg b1end b2beg b2end b3beg b3end b4beg b4end 1 78 *END 10. Simply Supported Thin Annular Plate (fine mesh) Keyword: *CONTROL_IMPLICIT_EIGENVALUE *CONTROL_IMPLICIT_GENERAL Description: A simply-supported annular plate of thickness t=0.06 m is to be analyzed to determine the first nine natural frequencies. The inner radius is 1.8 m and the outer radius is 6.0 m. This fine mesh analysis has 32 shell elements (circumferential) by 5 elements (radial). All nodes have = . On the outer nodes = = ZU = . A sketch representing the structure is shown below (Figure 10.1) along with the finite element model (Figure 10.2). Figure 10.2 – Fine mesh finite element model with simply supported boundary conditions on outer nodes. Analysis Summary: Dim. Type Load Material Geometry Contact Solver 3D Modal - Linear Linear - Implicit Solution Method Block Shift and Inverted Lanczos Units: kg, m, s, N, Pa, N-m (kilogram, meter, second, Newton, Pascal, Newton-meter) Dimensional Data: ro 6= , ri 8.1= , 06.0= Material Data: Mass Density Young's Modulus Poisson's Ratio ρ= = ν = Element Types: 11 × 8.00 10 × 2.00 10 0.3 /kg m Pa Fully integrated shell (elform=16) Material Models: *MAT_001 or *MAT_ELASTIC Results Comparison: LS-DYNA natural frequencies, first 10 (frequency in Hertz), and mode shapes (first 5) are compared with NAFEMS Natural Frequency Benchmark NF14. Mode(s) NAFEMS NF14 (Hz) Fine Mesh (Hz) 1 2, 3 4, 5 6 7, 8 9, 10 1.870 5.137 9.673 14.850 15.570 18.380 1.867 5.197 9.801 14.471 15.665 17.798 It is seen that with only a slight increase in mesh refinement, the LS-DYNA natural frequency results compare nicely with the NAFEMS Selected Benchmarks for Natural Eigenvalue Results: From the eigout file, generated by the *CONTROL_IMPLICIT_EIGENVALUE keyword: Simply Supported Thin Annular Plate (fine mesh) r e s u l t s o f e i g e n v a l u e a n a l y s i s: |------ frequency -----| MODE EIGENVALUE RADIANS CYCLES PERIOD 1 1.377019E+02 1.173465E+01 1.867627E+00 5.354388E-01 2 1.066283E+03 3.265399E+01 5.197045E+00 1.924171E-01 3 1.066283E+03 3.265399E+01 5.197045E+00 1.924171E-01 4 3.791946E+03 6.157878E+01 9.800567E+00 1.020349E-01 5 3.791946E+03 6.157878E+01 9.800567E+00 1.020349E-01 6 8.267193E+03 9.092411E+01 1.447102E+01 6.910362E-02 7 9.688143E+03 9.842836E+01 1.566536E+01 6.383511E-02 8 9.688143E+03 9.842836E+01 1.566536E+01 6.383511E-02 9 1.250545E+04 1.118278E+02 1.779794E+01 5.618626E-02 10 1.250545E+04 1.118278E+02 1.779794E+01 5.618626E-02 Mode Shapes (first three): Figures 10.3, 10.4, and 10.5 show the first 5 mode shapes with no contouring while Figures 10.6. 10.7, and 10.8 show the same 5 mode shapes with displacement contouring. Figure 10.4 - Modes 2 and 3, 5.197 Hz (NAFEMS 5.137) - no contouring. Figure 10.6 - Mode 1, 1.867 Hz (NAFEMS 1.870) - displacement contouring. Figure 10.8 - Modes 4 and 5, 9.801 Hz (NAFEMS 9.673) - displacement contouring. 72 *TITLE Simply Supported Thin Annular Plate (fine mesh) *CONTROL_IMPLICIT_EIGENVALUE $# neig center lflag lftend rflag rhtend eigmth shfscl 10 0.0 1 1.000000 1 30.00000 2 0.0 *CONTROL_IMPLICIT_GENERAL $# imflag dt0 imform nsbs igs cnstn form 1 1.000000 *CONTROL_TERMINATION $# endtim endcyc dtmin endeng endmas 1.000000 0 0.0 0.0 0.0 *DATABASE_BINARY_D3PLOT $# dt/cycl lcdt/nr beam npltc psetid 1.000000 *ELEMENT_SHELL $# eid pid n1 n2 n3 n4 n5 n6 n7 n8 1 1 1 33 34 2 192 1 192 224 193 161 *NODE $# nid x y z tc rc 1 1.79999995 0.0 0.0 224 5.88471174 -1.17054188 0.0 3 1 *BOUNDARY_SPC_SET $#nid/nsid cid dofx dofy dofz dofrx dofry dofrz 1 0 1 1 1 0 0 1 *BOUNDARY_SPC_SET $#nid/nsid cid dofx dofy dofz dofrx dofry dofrz 2 0 1 1 0 0 0 1 *PART $# title material type # 1 (Elastic) $# pid secid mid eosid hgid grav adpopt tmid 1 1 1 *SECTION_SHELL $# secid elform shrf nip propt qr/irid icomp setyp 1 6 0.0 0 1 0.0 0 1 $# t1 t2 t3 t4 nloc marea 0.060000 0.060000 0.060000 0.060000 0 0.0 *MAT_ELASTIC $# mid ro e pr da db not used 1 8000.0002.0000e+11 0.300000 0.0 0.0 0.0 *SET_NODE_LIST_GENERATE $# sid da1 da2 da3 da4 solver 1 0.0 0.0 0.0 0.0 $# b1beg b1end b2beg b2end b3beg b3end b4beg b4end 193 224 *SET_NODE_LIST_GENERATE $# sid da1 da2 da3 da4 solver 2 0.0 0.0 0.0 0.0 $# b1beg b1end b2beg b2end b3beg b3end b4beg b4end 1 192 *END 11. Transient Response to a Constant Force Keyword: *CONTROL_IMPLICIT_DYNAMICS *CONTROL_IMPLICIT_GENERAL *CONTROL_IMPLICIT_SOLVER *CONTROL_IMPLICIT_SOLUTION Description: A mass m=25.9067 lbf-s2/in is attached in the middle of a steel beam of length l=240 inches and geometric properties shown below. The beam is subjected to a dynamic load F(t) with a rise time of 0.075 seconds and a maximum constant value of 2000 pound- force. The weight of the beam is considered negligible. Determine the time of maximum displacement response tmax and the maximum displacement response ymax. Additionally, bendσ in the beam. The attached mass is modeled determine the maximum bending stress with a lumped mass element at the central node of the beam. A sketch representing the structure is shown below (Figure 11.1) along with the finite element model (Figure 11.2). Figure 11.2 – Finite element model with applied load (Node 12) and boundary conditions. In-plane boundary conditions and lumped mass (Node 12) are not shown. Analysis Summary: Dim. Type Load Material Geometry Contact Solver 3D Dynamic Force Linear Linear - Implicit Solution Method 2-Nonlinear w/BFGS Units: lbf-s2/in, in, s, lbf, psi, lbf-in (blob, inch, second, pound force, pound force/inch2, pound force-inch) Dimensional Data: = 240.0 in , = 18.0 in , zI = 800.6 in As a cross-section-integrated beam is used, the cross sectional dimension is calculated. , a thickness of Given is obtained. 800.6 1.647 and 18.0 in in in = = = Material Data: Mass Density Young's Modulus Poisson's Ratio Nodal Mass = = ν = = Load: − 20 lbf − / in × 1.0 10 × 3.0 10 0.3 25.9067 psi blobs Lateral Load F t = ( ) *DEFINE_CURVE Element Types: Hughes-Liu beam with cross section integration (elform=1) Lumped mass (*ELEMENT_MASS entry) Material Models: *MAT_001 or *MAT_ELASTIC Results Comparison: LS-DYNA results for time of the maximum displacement response tmax, the maximum σ in the beam are displacement response ymax, and the maximum bending stress compared with J.M. Biggs' studies in Introduction to Structural Dynamics (pg. 50). bend Time - tmax (s) Disp. - ymax (in) Stress - σ (psi) bend Biggs 0.0920 0.3310 1.8600 10× Node 12/Element 10 0.0930 0.3421 1.8151 10× These nodal time/displacement results (Figure 11.3) were generated by *DATABASE_ NODOUT keyword while the element stress results (Figure 11.4) were generated by *DATABASE_ELOUT. Lobatto integration (qr=4 - 3×3 quadrature - *SECTION_BEAM) was employed since it has an advantage in that the inner and outer integration points are on the beam surfaces. Gauss integration is the default quadrature rule (qr=2 - 2×2 quadrature - *SECTION_ BEAM). The contour plots of the axial beam stresses for the upper (ip=1) and lower (ip=3) surfaces of the beam (Figure 11.5) were obtained from the d3plot file at t=0.093 s which were generated by the *DATABASE_BINARY_D3PLOT keyword. Figure 11.4 – Axial beam stress vs. time at the upper (ip=1), the point of maximum bending stress, and the lower (ip=3) beam surfaces for Element 10. Figure 11.5 – Contour plots of the axial beam stresses for the upper (ip=1) *TITLE Transient Response to a Constant Force *CONTROL_IMPLICIT_DYNAMICS $# imass gamma beta 1 0.500000 0.250000 *CONTROL_IMPLICIT_GENERAL $# imflag dt0 imform nsbs igs cnstn form 1 0.001000 2 1 2 *CONTROL_IMPLICIT_SOLVER $# lsolvr lprint negev order drcm drcprm autospc autotol 4 2 2 0 1 0.0 1 0.0 $# lcpack 2 *CONTROL_IMPLICIT_SOLUTION $# nsolvr ilimit maxref dctol ectol rctol lstol abstol 2 11 15 0.0010 0.0100 1.00e+10 0.900000 1.00e-10 $# dnorm diverg istif nlprint 2 1 1 2 $# arcctl arcdir arclen arcmth arcdmp 0 1 0.0 1 2 *CONTROL_TERMINATION $# endtim endcyc dtmin endeng endmas 0.100000 0 0.900000 0.0 0.0 *DATABASE_ELOUT $# dt binary 1.0000e-05 1 *DATABASE_MATSUM $# dt binary 1.0000e-05 1 *DATABASE_NODOUT $# dt binary 1.0000e-05 1 *DATABASE_SPCFORC $# dt binary 1.0000e-05 1 *DATABASE_BINARY_D3PLOT $# dt/cycl lcdt/nr beam npltc psetid 1.0000e-05 *DATABASE_BINARY_D3THDT $# dt/cycl lcdt/nr beam npltc psetid 2.0000e-04 *DATABASE_EXTENT_BINARY $# neiph neips maxint strflg sigflg epsflg rltflg engflg 0 0 0 0 1 1 1 1 $# cmpflg ieverp beamip dcomp shge stssz n3thdt ialemat 0 0 20 1 1 1 2 *DATABASE_HISTORY_NODE $# nid1 nid2 nid3 nid4 ni5 nid6 nid7 nid8 12 1 2 *DATABASE_HISTORY_BEAM $# eid1 eid2 eid3 eid4 ei5 eid6 eid7 eid8 10 11 *DEFINE_CURVE $# lcid sdir sfa sfo offa offo dattyp 1 0 1.000000 1.000000 0.0 0.0 $# a1 o1 0.0 0.0 0.07500000 2.0000000e+04 1.00000000 2.0000000e+04 *ELEMENT_BEAM $# eid pid n1 n2 n3 n4 n5 n6 n7 n8 1 1 1 3 22 20 1 21 2 41 *ELEMENT_MASS $# eid id mass pid 1 0.0 0.0 0.0 41 234.0000000 0.0 0.99996525 *BOUNDARY_SPC_SET $#nid/nsid cid dofx dofy dofz dofrx dofry dofrz 2 0 1 1 1 1 1 *BOUNDARY_SPC_SET $#nid/nsid cid dofx dofy dofz dofrx dofry dofrz 3 0 0 0 1 1 1 *PART $# title Part 1 for Mat 1 and Elem Type 1 $# pid secid mid eosid hgid grav adpopt tmid 1 1 1 *SECTION_BEAM $# secid elform shrf qr/irid cst scoor 1 1 0.830000 4 0 0.0 $# ts1 ts2 tt1 tt2 nsloc ntloc 1.647220 1.647220 18.0 18.0 *MAT_ELASTIC $# mid ro e pr da db not used 11.0000e-203.0000e+07 0.300000 0.0 0.0 0.0 *LOAD_NODE_SET $# nsid dof lcid sf cid m1 m2 m3 1 2 1 1.000000 *SET_NODE_LIST $# sid da1 da2 da3 da4 solver 1 0.0 0.0 0.0 0.0 $# nid1 nid2 nid3 nid4 nid5 nid6 nid7 nid8 12 *SET_NODE_LIST $# sid da1 da2 da3 da4 solver 2 0.0 0.0 0.0 0.0 $# nid1 nid2 nid3 nid4 nid5 nid6 nid7 nid8 1 2 *SET_NODE_LIST $# sid da1 da2 da3 da4 solver 3 0.0 0.0 0.0 0.0 $# nid1 nid2 nid3 nid4 nid5 nid6 nid7 nid8 3 4 5 6 7 8 9 10 11 12 13 14 15 16 17 18 19 20 21 22 23 24 25 26 27 28 29 30 31 32 33 34 35 36 37 38 39 40 41 *END 12. Simply Supported Square Plate: Out-of-Plane Vibration (solid mesh) Keywords: *CONTROL_IMPLICIT_EIGENVALUE *CONTROL_IMPLICIT_GENERAL Description: Determine the first 10 natural frequencies of a solid simply-supported plate of thickness t=1.0 m. Each side of the plate measure 10.0 m. The plate is meshed with solid hexahedra element with an 8 x 8 x 3 density. On the lower surface, outer boundary nodes, ZU = . The finite element model is shown in Figure 12.1. Figure 12.1 – Finite element model with simply supported Analysis Summary: Dim. Type Load Material Geometry Contact Solver 3D Modal - Linear Linear - Implicit Solution Method Block Shift and Inverted Lanczos Units: kg, m, s, N, Pa, N-m (kilogram, meter, second, Newton, Pascal, Newton-meter) Dimensional Data: Rectangular dimensions of square plate: 10.0 m x 10.0 m x 1.00 m. Material Data: Mass Density Young's Modulus Poisson's Ratio ρ= = ν = Element Types: 11 × 8.00 10 × 2.00 10 0.3 /kg m Pa Constant stress solid (elform=1) Fully integrated S/R solid (elform=2) Fully integrated S/R solid - for poor aspect ratio (eff) - (elform=-1) Fully integrated S/R solid - for poor aspect ratio (acc) - (elform=-2) Fully integrated quadratic 8 node element with nodal rotations (elform=3) Material Models: *MAT_001 or *MAT_ELASTIC Results Comparison: LS-DYNA natural frequencies, first 10 (frequency in Hertz), and mode shapes (4 through Mode(s) NAFEMS FV52 (Hz) elform=1 (Hz) elform=2 (Hz) elform=-1 (Hz) elform=-2 (Hz) elform=3 (Hz) 1, 2, 3 rigid body rigid body rigid body rigid body rigid body rigid body 4 45.897 44.040 48.508 45.448 46.2060 43.370 5, 6 109.440 106.468 120.388 107.114 109.265 104.703 7 8 9 167.890 155.523 169.601 159.102 163.943 153.862 193.590 193.582 193.526 193.518 193.526 193.227 206.190 200.135 200.188 198.791 200.176 196.485 10 206.190 200.135 200.188 198.873 200.176 197.280 Hourglass control (*HOURGLASS) is necessary for the constant stress solid (elform=1) element formulation (the LS-DYNA default), especially at higher frequencies. Only this element formulation (elform=1) makes use of this feature The constant stress solid (elform=1), the fully integrated S/R solid (elform=2), and the fully integrated quadratic 8 node element with nodal rotations (elform=3) all provide similar frequency results for this analysis. The fully integrated quadratic 8 node element with nodal rotations (elform=3) formulation provides two distinct modes and frequencies for modes 9 and 10, whereas, all the other formulations provide the same results for modes 9 and 10. This is perhaps due to the accountability of the nodal rotations. The aspect ratio of these elements is 3.75 (ratio of side to depth length). It would, however, for this frequency analysis, appear that the element formulations available to address poor aspect ratios (elform=-1 or -2) do not offer much improvement. The constant stress solid (elform=1), the fully integrated S/R solid (elform=2), and the fully integrated quadratic 8 node element with nodal rotations (elform=3) formulation all appear to provide more than adequate results for this frequency study. The fully integrated S/R solid (the efficient formulation choice) intended to address poor aspect ratios (elform=-1), provided somewhat different shapes for modes 9 and 10. This stiffness reduction for certain modes (according to Borrvall [2009]). However, modes 9 and 10 are not those modes Borrvall offered concerns for in stiffness reduction. Eigenvalue Results: From the eigout file, generated by the *CONTROL_IMPLICIT_EIGENVALUE keyword: Constant stress solid (elform=1): Simply Supported Square Plate: Out-of-Plane Vibration r e s u l t s o f e i g e n v a l u e a n a l y s i s: |------ frequency -----| MODE EIGENVALUE RADIANS CYCLES PERIOD 1 -3.201421E-10 1.789252E-05 2.847682E-06 3.511628E+05 2 1.062290E-09 3.259279E-05 5.187303E-06 1.927784E+05 3 2.881279E-09 5.367755E-05 8.543047E-06 1.170543E+05 4 7.657028E+04 2.767133E+02 4.404030E+01 2.270648E-02 5 4.475080E+05 6.689604E+02 1.064684E+02 9.392462E-03 6 4.475080E+05 6.689604E+02 1.064684E+02 9.392462E-03 7 9.548827E+05 9.771810E+02 1.555232E+02 6.429910E-03 8 1.479411E+06 1.216310E+03 1.935818E+02 5.165775E-03 9 1.581263E+06 1.257483E+03 2.001346E+02 4.996637E-03 10 1.581263E+06 1.257483E+03 2.001346E+02 4.996637E-03 Fully integrated S/R solid (elform=2) Simply Supported Square Plate: Out-of-Plane Vibration r e s u l t s o f e i g e n v a l u e a n a l y s i s: |------ frequency -----| MODE EIGENVALUE RADIANS CYCLES PERIOD 1 -6.009941E-09 7.752381E-05 1.233830E-05 8.104846E+04 2 9.895302E-10 3.145680E-05 5.006505E-06 1.997401E+05 3 5.558832E-09 7.455757E-05 1.186621E-05 8.427293E+04 4 9.289190E+04 3.047817E+02 4.850752E+01 2.061536E-02 5 5.721748E+05 7.564224E+02 1.203884E+02 8.306451E-03 6 5.721748E+05 7.564224E+02 1.203884E+02 8.306451E-03 7 1.135577E+06 1.065635E+03 1.696010E+02 5.896191E-03 8 1.478563E+06 1.215962E+03 1.935263E+02 5.167257E-03 9 1.582107E+06 1.257818E+03 2.001880E+02 4.995304E-03 10 1.582107E+06 1.257818E+03 2.001880E+02 4.995304E-03 Fully integrated S/R solid - for poor aspect ratio (eff) - (elform=-1) Simply Supported Square Plate: Out-of-Plane Vibration r e s u l t s o f e i g e n v a l u e a n a l y s i s: |------ frequency -----| MODE EIGENVALUE RADIANS CYCLES PERIOD 1 1.043372E-08 1.021456E-04 1.625698E-05 6.151205E+04 2 1.335866E-08 1.155797E-04 1.839507E-05 5.436238E+04 3 1.573062E-08 1.254218E-04 1.996149E-05 5.009645E+04 4 8.154482E+04 2.855605E+02 4.544837E+01 2.200299E-02 5 4.529502E+05 6.730158E+02 1.071138E+02 9.335866E-03 6 4.529502E+05 6.730158E+02 1.071138E+02 9.335866E-03 7 9.993359E+05 9.996679E+02 1.591021E+02 6.285273E-03 8 1.478432E+06 1.215908E+03 1.935178E+02 5.167484E-03 9 1.560100E+06 1.249040E+03 1.987908E+02 5.030413E-03 Fully integrated S/R solid - for poor aspect ratio (acc) - (elform=-2) Simply Supported Square Plate: Out-of-Plane Vibration r e s u l t s o f e i g e n v a l u e a n a l y s i s: |------ frequency -----| MODE EIGENVALUE RADIANS CYCLES PERIOD 1 2.211891E-09 4.703075E-05 7.485176E-06 1.335974E+05 2 7.014023E-09 8.374977E-05 1.332919E-05 7.502332E+04 3 1.121953E-08 1.059223E-04 1.685805E-05 5.931883E+04 4 8.428602E+04 2.903205E+02 4.620595E+01 2.164223E-02 5 4.713255E+05 6.865315E+02 1.092649E+02 9.152072E-03 6 4.713255E+05 6.865315E+02 1.092649E+02 9.152072E-03 7 1.061078E+06 1.030087E+03 1.639434E+02 6.099667E-03 8 1.478558E+06 1.215960E+03 1.935260E+02 5.167264E-03 9 1.581923E+06 1.257745E+03 2.001764E+02 4.995595E-03 10 1.581923E+06 1.257745E+03 2.001764E+02 4.995595E-03 Fully integrated quadratic 8 node element with nodal rotations (elform=3) Simply Supported Square Plate r e s u l t s o f e i g e n v a l u e a n a l y s i s: |------ frequency -----| MODE EIGENVALUE RADIANS CYCLES PERIOD 1 1.877197E-08 1.370108E-04 2.180595E-05 4.585904E+04 2 2.239540E-08 1.496509E-04 2.381768E-05 4.198561E+04 3 2.614979E-08 1.617090E-04 2.573678E-05 3.885490E+04 4 7.425572E+04 2.724990E+02 4.336957E+01 2.305764E-02 5 4.327897E+05 6.578675E+02 1.047029E+02 9.550837E-03 6 4.327897E+05 6.578675E+02 1.047029E+02 9.550837E-03 7 9.345968E+05 9.667455E+02 1.538623E+02 6.499317E-03 8 1.473997E+06 1.214083E+03 1.932273E+02 5.175253E-03 9 1.524111E+06 1.234549E+03 1.964846E+02 5.089458E-03 10 1.536475E+06 1.239546E+03 1.972799E+02 5.068940E-03 Mode Shapes: The constant stress solid (elform=1) mode shapes are shown in Figure 12.2, the fully integrated S/R solid (elform=2) in Figure 12.3, the fully integrated quadratic 8 node element with nodal rotations (elform=3) in Figure 12.4, the fully integrated S/R solid (the so-called efficient formulation choice) intended to address poor aspect ratios (elform=-1) in Figure 12.5, and the fully integrated S/R solid (the so-called accurate formulation choice) intended to address poor aspect ratios (elform=-2) in Figure 12.6. The first three modes are not shown (rigid body translations). Modes 4 through 10 are shown for the selected results. Modes 5 and 6 are identical for all element formulations; modes 9 and 10 are also identical for all, with the exception of the fully integrated Figure 12.2 - Mode shapes for constant stress solid (elform=1). Figure 12.4 - Mode shapes for fully integrated quadratic 8 node element with nodal rotations (elform=3). Figure 12.6 - Mode shapes fully integrated S/R solid (elform=-2). Input deck: *KEYWORD *TITLE Simply Supported Square Plate: Out-of-Plane Vibration (solid mesh) *CONTROL_IMPLICIT_EIGENVALUE $# neig center lflag lftend rflag rhtend eigmth shfscl 10 0.0 0 0.0 0 0.0 0 0.0 *CONTROL_IMPLICIT_GENERAL $# imflag dt0 imform nsbs igs cnstn form 1 0.0 *CONTROL_TERMINATION $# endtim endcyc dtmin endeng endmas 1.000000 0 0.0 0.0 0.0 *DATABASE_BINARY_D3PLOT $# dt/cycl lcdt/nr beam npltc psetid 1.000000 *ELEMENT_SOLID $# eid pid n1 n2 n3 n4 n5 n6 n7 n8 1 1 1 37 41 5 2 38 42 6 192 1 283 319 323 287 284 320 324 288 *NODE $# nid x y z tc rc 1 0.0 0.0 0.0 3 324 10.00000000 10.00000000 1.00000000 *BOUNDARY_SPC_SET $#nid/nsid cid dofx dofy dofz dofrx dofry dofrz 1 0 0 0 1 *PART $# title material type # 1 (Elastic) $# secid elform aet 1 1 1 $ 1 2 1 $ 1 -1 1 $ 1 -2 1 $ 1 3 1 *MAT_ELASTIC $# mid ro e pr da db not used 1 8000.0002.0000e+11 0.300000 0.0 0.0 0.0 *HOURGLASS $# hgid ihq qm ibq q1 q2 qb qw 1 6 1.0 0 0.0 0.0 0.0 0.0 *SET_NODE_LIST $# sid da1 da2 da3 da4 solver 1 0.0 0.0 0.0 0.0 $# nid1 nid2 nid3 nid4 nid5 nid6 nid7 nid8 1 37 73 109 145 181 217 253 289 293 297 301 305 309 313 317 321 285 249 213 177 141 105 69 33 29 25 21 17 13 9 5 *END 13. Simply Supported Square Plate: Out-of-Plane Vibration (thick shell mesh) Keywords: *CONTROL_IMPLICIT_EIGENVALUE *CONTROL_IMPLICIT_GENERAL Description: Determine the first 10 natural frequencies of a solid simply-supported plate of thickness t=1.0 m. Each side of the plate measure 10.0 m. The plate is meshed with solid hexahedra element with an 8 x 8 x 3 density. On the lower surface, outer boundary nodes, ZU = . The finite element model is shown in Figure 13.1. Figure 13.1 – Finite element model with simply supported Analysis Summary: Dim. Type Load Material Geometry Contact Solver 3D Modal - Linear Linear - Implicit Solution Method Block Shift and Inverted Lanczos Units: kg, m, s, N, Pa, N-m (kilogram, meter, second, Newton, Pascal, Newton-meter) Dimensional Data: Rectangular dimensions of square plate: 10.0 m x 10.0 m x 1.00 m. Material Data: Mass Density Young's Modulus Poisson's Ratio ρ= = ν = Element Types: 11 × 8.00 10 × 2.00 10 0.3 /kg m Pa S/R 2x2 IPI thick shell (elform=2) Assumed strain 2x2 IPI thick shell (elform=3) Assumed strain RI thick shell (elform=5) Material Models: *MAT_001 or *MAT_ELASTIC Results Comparison: LS-DYNA natural frequencies, first 10 (frequency in Hertz), and mode shapes (4 through Mode(s) NAFEMS FV52 (Hz) elform=2 (Hz) elform=3 (Hz) elform=5 (Hz) 1, 2, 3 rigid body rigid body rigid body rigid body 4 45.897 43.480 42.556 44.656 5, 6 109.440 105.363 102.983 107.290 7 8 9 167.890 152.764 150.187 157.397 193.590 185.301 193.378 193.583 206.190 193.708 197.247 200.136 10 206.190 200.997 197.295 200.136 The assumed strain 2x2 IPI thick shell (elform=3) and the assumed strain RI thick shell (elform=5) use a full three-dimensional stress update rather than the two-dimensional plane stress update of the one point reduced integration (elform=1) and the selectively reduced 2x2 IPI thick shell (elform=2). The selectively reduced 2x2 IPI thick shell (elform=2), the assumed strain 2x2 IPI thick shell (elform=3), and the assumed strain RI thick shell (elform=5) all provide similar frequency results for this analysis. The selectively reduced 2x2 IPI thick shell (elform=2) formulation appears to have identified (added) an unexpected result for mode 8 (an anomaly, a low energy warping mode which is believed will not cause solution troubles) due to the calculation of the out- of-plane shear stiffness terms. Code inspection indicated that the out-of-plane shear stress and stiffness is calculated at the mid-point rather than the 2x2 integration points in order to prevent shear locking in bending. Modes 9 and 10 (elform=2) are however, similar to modes 8 and 9, respectively, for the assumed strain RI thick shell (elform=5) formulation. The assumed strain 2x2 IPI thick shell (elform=3) formulation appears to have identified two different modes and frequencies for modes 9 and 10. This is possibly due to the employment of a corotational system that rotates with the elements, which suppresses the Eigenvalue Results: From the eigout file, generated by the *CONTROL_IMPLICIT_EIGENVALUE keyword: S/R 2x2 IPI thick shell (elform=2) Simply Supported Square Plate: Out-of-Plane Vibration (thick shell mesh) r e s u l t s o f e i g e n v a l u e a n a l y s i s: |------ frequency -----| MODE EIGENVALUE RADIANS CYCLES PERIOD 1 -8.469215E-09 9.202834E-05 1.464676E-05 6.827446E+04 2 -3.463356E-09 5.885028E-05 9.366313E-06 1.067656E+05 3 -1.746230E-09 4.178791E-05 6.650753E-06 1.503589E+05 4 7.449258E+04 2.729333E+02 4.343868E+01 2.302096E-02 5 4.377512E+05 6.616277E+02 1.053013E+02 9.496558E-03 6 4.377512E+05 6.616277E+02 1.053013E+02 9.496558E-03 7 9.193747E+05 9.588403E+02 1.526042E+02 6.552901E-03 8 1.255008E+06 1.120271E+03 1.782967E+02 5.608628E-03 9 1.481334E+06 1.217101E+03 1.937076E+02 5.162420E-03 10 1.594925E+06 1.262903E+03 2.009973E+02 4.975191E-03 Assumed strain 2x2 IPI thick shell (elform=3) Simply Supported Square Plate: Out-of-Plane Vibration (thick shell mesh) r e s u l t s o f e i g e n v a l u e a n a l y s i s: |------ frequency -----| MODE EIGENVALUE RADIANS CYCLES PERIOD 1 -8.338247E-09 9.131400E-05 1.453308E-05 6.880856E+04 2 -4.802132E-09 6.929742E-05 1.102903E-05 9.066983E+04 3 -3.012246E-09 5.488394E-05 8.735050E-06 1.144813E+05 4 7.149598E+04 2.673873E+02 4.255601E+01 2.349844E-02 5 4.186854E+05 6.470590E+02 1.029826E+02 9.710374E-03 6 4.186854E+05 6.470590E+02 1.029826E+02 9.710374E-03 7 8.904817E+05 9.436534E+02 1.501871E+02 6.658361E-03 8 1.476299E+06 1.215030E+03 1.933781E+02 5.171217E-03 9 1.535967E+06 1.239341E+03 1.972473E+02 5.069778E-03 10 1.536702E+06 1.239638E+03 1.972945E+02 5.068565E-03 Assumed strain RI thick shell (elform=5) Simply Supported Square Plate: Out-of-Plane Vibration (thick shell mesh) r e s u l t s o f e i g e n v a l u e a n a l y s i s: |------ frequency -----| MODE EIGENVALUE RADIANS CYCLES PERIOD 1 5.966285E-10 2.442598E-05 3.887516E-06 2.572337E+05 2 2.881279E-09 5.367755E-05 8.543047E-06 1.170543E+05 3 5.762558E-09 7.591152E-05 1.208169E-05 8.276986E+04 4 7.872674E+04 2.805829E+02 4.465615E+01 2.239333E-02 5 4.544420E+05 6.741231E+02 1.072900E+02 9.320531E-03 6 4.544420E+05 6.741231E+02 1.072900E+02 9.320531E-03 7 9.780258E+05 9.889519E+02 1.573966E+02 6.353378E-03 8 1.479432E+06 1.216319E+03 1.935832E+02 5.165738E-03 9 1.581277E+06 1.257488E+03 2.001355E+02 4.996615E-03 Mode Shapes: The first three modes are not shown (rigid body translations). Modes 4 through 10 are shown for the selected results. Modes 5 and 6 are identical for all element formulations. Modes 9 and 10 offer three different sets of results, depending on element formulation; (1) for selectively reduced 2x2 IPI thick shell (elform=2), there is a distinct difference in natural frequencies (Figure 13.2), (2) for assumed strain 2x2 IPI thick shell (elform=3), there is a very slight difference (Figure 13.3), and (3) for assumed strain RI thick shell (elform=5), the results are identical (Figure 13.4). Figure 13.3 - Mode shapes for assumed strain 2x2 IPI thick shell (elform=3). *TITLE Simply Supported Square Plate: Out-of-Plane Vibration (thick shell mesh) *CONTROL_IMPLICIT_EIGENVALUE $# neig center lflag lftend rflag rhtend eigmth shfscl 10 0.0 0 0.0 0 0.0 0 0.0 *CONTROL_IMPLICIT_GENERAL $# imflag dt0 imform nsbs igs cnstn form 1 0.0 *CONTROL_SHELL $# wrpang esort irnxx istupd theory bwc miter proj 20.00000 0 0 0 2 2 1 $# rotascl intgrd lamsht cstyp6 tshell nfail1 nfail4 0.0 1 *CONTROL_TERMINATION $# endtim endcyc dtmin endeng endmas 1.000000 0 0.0 0.0 0.0 *DATABASE_BINARY_D3PLOT $# dt/cycl lcdt/nr beam npltc psetid 1.000000 *ELEMENT_TSHELL $# eid pid n1 n2 n3 n4 n5 n6 n7 n8 1 1 1 37 41 5 2 38 42 6 192 1 283 319 323 287 284 320 324 288 *NODE $# nid x y z tc rc 1 0.0 0.0 0.0 3 324 10.00000000 10.00000000 1.00000000 *BOUNDARY_SPC_SET $#nid/nsid cid dofx dofy dofz dofrx dofry dofrz 1 0 0 0 1 *PART $# title material type # 1 (Elastic) $# pid secid mid eosid hgid grav adpopt tmid 1 1 1 0 1 *SECTION_TSHELL $# secid elform shrf nip propt qr/irid icomp tshear 1 2 0.0 5 0 0.0 $ 1 3 0.0 5 0 0.0 $ 1 5 0.0 5 0 0.0 *MAT_ELASTIC $# mid ro e pr da db not used 1 8000.0002.0000e+11 0.300000 0.0 0.0 0.0 *HOURGLASS $# hgid ihq qm ibq q1 q2 qb qw 1 4 0.1 0 0.0 0.0 0.0 0.0 *SET_NODE_LIST $# sid da1 da2 da3 da4 solver 1 0.0 0.0 0.0 0.0 $# nid1 nid2 nid3 nid4 nid5 nid6 nid7 nid8 1 37 73 109 145 181 217 253 289 293 297 301 305 309 313 317 321 285 249 213 177 141 105 69 33 29 25 21 17 13 9 5 *END Notes: 1. The assumed strain 2x2 IPI thick shell (elform=3) and the assumed strain RI thick shell (elform=5) are distortion sensitive and should not be used in situations where 2. With the one point reduced integration (elform=1) and the selectively reduced 2x2 IPI thick shell (elform=2), a single element through the thickness will capture bending response, but with the assumed strain 2x2 IPI thick shell (elform=3) and the assumed strain RI thick shell (elform=5), two elements are recommended to avoid excessive softness. 3. Only the selectively reduced 2x2 IPI thick shell (elform=2), the assumed strain 2x2 IPI thick shell (elform=3), and the assumed strain RI thick shell (elform=5) are available for implicit applications. If one point reduced integration (elform=1) is specified in an implicit analysis, it is internally switched to selectively reduced 2x2 14. Simply Supported Square Plate: Transient Forced Vibration (solid mesh) Keywords: *CONTROL_IMPLICIT_AUTO *CONTROL_IMPLICIT_DYNAMICS *CONTROL_IMPLICIT_GENERAL *CONTROL_IMPLICIT_SOLVER *CONTROL_IMPLICIT_SOLUTION Description: A plate is subjected to a suddenly applied pressure on its top. A transient analysis is performed in order to obtain the response of the plate. Damping is present. On the lower surface, outer boundary nodes, ZU = . The finite element model is shown in Figure 14.1. Figure 14.1 – Finite element model with applied pressure on upper surface and Analysis Summary: Dim. Type Load Material Geometry Contact Solver Solution Method 3D Dynamic Pressure Damping Linear Linear - Implicit 1 - Linear Units: kg, m, s, N, Pa, N-m (kilogram, meter, second, Newton, Pascal, Newton-meter) Dimensional Data: Rectangular dimensions of square plate: 10.0 m x 10.0 m x 1.00 m. Material Data: Mass Density Young's Modulus Poisson's Ratio Damping ratio Load: Pressure Element Types: /kg m Pa 11 ρ= × 8.00 10 × = 2.00 10 ν = 0.3 %2=ζ = × 1.0 10 Pa Constant stress solid (elform=1) Fully integrated S/R solid (elform=2) Fully integrated S/R solid - for poor aspect ratio (eff) - (elform=-1) Fully integrated S/R solid - for poor aspect ratio (acc) - (elform=-2) Fully integrated quadratic 8 node element with nodal rotations (elform=3) Material Models: *MAT_001 or *MAT_ELASTIC Damping: id ωζ2= As the excited mode is the first, corresponding to ) (that from NAFEMS Benchmark Test FV52), we choose the damping factor relative to the first frequency: 288.380 45.897 rad s Hz ( / ω = = 1 11.535 = Hz Results Comparison: LS-DYNA X-direction bending stress, σxx , at (Node 161) on bottom surface plus its Z- displacement, ZU , are compared with NAFEMS Selected Benchmarks for Forced Vibration, Test 21T. Reference Condition - Center (Node 161) Peak Bending Stress σxx (Pa) Peak ZU (m) Steady-State ZU (m) NAFEMS Benchmark Test 21T 6.211 10× 4.524 10− × − 2.333 10− × − Constant stress solid (elform=1) 4.638 10× 5.438 10− × − 2.778 10− × − Fully integrated S/R solid (elform=2) Fully integrated S/R solid (elform=-1) Fully integrated S/R solid (elform=-2) 3.732 10× 3.925 10− × − 2.019 10− × − 4.611 10× 4.435 10− × − 2.242 10− × − 4.221 10× 4.365 10− × − 2.203 10− × − Fully integrated quadratic element with nodal rotations (elform=3) x xxx × . 10 − x xxx . × 10 − − x xxx . × 10 − The constant stress solid (elform=1) result of × 4.638 10 Pa is an element centroid value. These nodal displacement results were generated by *DATABASE_NODOUT keyword while the axial stress (nodal) results were generated by *DATABASE_ELOUT (elout file) and *DATABASE_EXTENT_BINARY (eloutdet file provides detailed element output at integration points and connectivity nodes) keyword entries. You can set intout=stress or intout=all (*DATABASE_EXTENT_BINARY) and have file called eloutdet integration points stresses output for all to a (*DATABASE_ELOUT governs the output interval and *DATABASE_HISTORY_ SOLID governs which elements are output). Setting nodout=stress or nodout=all in *DATABASE_EXTENT_BINARY will write the extrapolated nodal stresses to eloutdet. LS-DYNA stress and strain output corresponds to integration point locations. Stress at a node is an artifact of the post-processor and represents an average of the surrounding integration point stresses (the value will likely be different with different post- processors). For this coarse mesh, the one-point quadrature (low order) constant stress solid (elform=1) element formulation (the LS-DYNA default) provides a less stiff, stress and displacement comparison. Refinement of the mesh should provide a better comparison. The higher order, fully integrated selectively reduced solid (elform=2) provides a comparatively stiff result, both in stress and displacement, probably due to the coarse mesh. The aspect ratio of these elements is 3.75 (ratio of side to depth length). Available options are the higher order, fully integrated S/R solid (both the so-called efficient and the so-called accurate formulation choices) intended to address poor aspect ratios (elform=-1 and -2, respectively). These formulations provide a good comparison of displacements (peak and steady-state) for this coarse mesh. Unfortunately, the stress comparison is not very good; it is not understood why at this time. The fully integrated S/R solid (the so-called efficient formulation choice) intended to address poor aspect ratios (elform=-1), can provide a slightly less stiff solution than the so-called accurate formulation choice (elform=2). This formulation (elform=-1) involves a slight modification of the Jacobian matrix which can lead to a stiffness reduction for certain modes, in particular the out-of-plane hourglass mode (according to Borrvall [2009]). The higher order, fully integrated quadratic 8 node element with nodal rotations (elform=3) formulation provides a (????) results. Waiting for LSTC LS-DYNA code fix to remark on this. For the fully integrated S/R solid accurate formulation (elform=-2), the contour plot of the X-direction bending stress (Figure 14.2) and the Z-displacement (Figure 14.3) were obtained from the d3plot file at peak displacement time which were generated by the Figure 14.2 – Contour plot of the X-stress (elform=-2) at peak displacement time. *TITLE Simply Supported Square Plate: Transient Forced Vibration (solid mesh) *CONTROL_IMPLICIT_AUTO $# iauto iteopt itewin dtmin dtmax dtexp kfail kcycle 0 11 5 0.0 0.0 *CONTROL_IMPLICIT_DYNAMICS $# imass gamma beta 1 0.500000 0.250000 *CONTROL_IMPLICIT_GENERAL $# imflag dt0 imform nsbs igs cnstn form zero_v 1 0.000100 2 1 2 *CONTROL_IMPLICIT_SOLVER $# lsolvr lprint negev order drcm drcprm autospc autotol 4 2 2 0 1 0.0 1 0.0 $# lcpack 2 *CONTROL_IMPLICIT_SOLUTION $# nsolvr ilimit maxref dctol ectol rctol lstol abstol 2 11 15 0.0010 0.0100 1.00e+10 0.900000 1.000000 $# dnorm diverg istif nlprint 2 1 1 2 $# arcctl arcdir arclen arcmth arcdmp 0 1 0.0 1 2 *CONTROL_TERMINATION $# endtim endcyc dtmin endeng endmas 0.020000 0 0.0 0.0 0.0 *DATABASE_ELOUT $# dt binary lcur ioopt 1.0000e-06 1 *DATABASE_NODFOR $# dt binary lcur ioopt 1.0000e-06 1 *DATABASE_NODOUT $# dt binary lcur ioopt 1.0000e-06 1 *DATABASE_BINARY_D3PLOT $# dt/cycl 0.001000 *DATABASE_EXTENT_BINARY $# neiph neips maxint strflg sigflg epsflg rtflg engflg $# cmpflg ieverp beamip dcomp shge stssz n3thdt ialemat $# nintsld pkp_sen sclp hydro msscl therm intout nodout 8 1.0 stress stress *DATABASE_HISTORY_SOLID $# id1 id2 id3 id4 id5 id6 id7 id8 28 29 36 37 *DATABASE_NODAL_FORCE_GROUP $# nsid cid 164 *DATABASE_HISTORY_NODE $# nid1 nid2 nid3 nid4 nid5 nid6 nid7 nid8 161 164 *SET_NODE_LIST $# sid da1 da2 da3 da4 solver 164 0.0 0.0 0.0 0.0 $# nid1 nid2 nid3 nid4 nid5 nid6 nid7 nid8 164 *DAMPING_GLOBAL $# lcid valdmp stx sty stz srx sry srz 0 11.53500 0.0 0.0 0.0 0.0 0.0 0.0 *DEFINE_CURVE $# lcid sdir sfa sfo offa offo dattyp 1 0 0.0 0.0 0.0 0.0 $# a1 o1 $# eid pid n1 n2 n3 n4 n5 n6 n7 n8 1 1 1 37 41 5 2 38 42 6 192 1 283 319 323 287 284 320 324 288 *NODE $# nid x y z tc rc 1 0.0 0.0 0.0 3 324 10.00000000 10.00000000 1.00000000 *BOUNDARY_SPC_SET $#nid/nsid cid dofx dofy dofz dofrx dofry dofrz 1 0 0 0 1 *PART $# title material type # 1 (Elastic) $# pid secid mid eosid hgid grav adpopt tmid 1 1 1 *SECTION_SOLID $# secid elform aet 1 1 1 $ 1 2 1 $ 1 -1 1 $ 1 -2 1 $ 1 3 1 *MAT_ELASTIC $# mid ro e pr da db not used 1 8000.0002.0000e+11 0.300000 0.0 0.0 0.0 *LOAD_SEGMENT $# lcid sf at n1 n2 n3 n4 1 1.000000 0.0 4 40 44 8 1 1.000000 0.0 284 320 324 288 *SET_NODE_LIST $# sid da1 da2 da3 da4 solver 1 0.0 0.0 0.0 0.0 $# nid1 nid2 nid3 nid4 nid5 nid6 nid7 nid8 1 37 73 109 145 181 217 253 289 293 297 301 305 309 313 317 321 285 249 213 177 141 105 69 33 29 25 21 17 13 9 5 *END Notes: 1. One should remember that the constant stress solid (elform=1), the fully integrated S/R solid (elform=2), and the fully integrated S/R solid (both the so-called efficient and the so-called accurate formulation choices) intended to address poor aspect ratios (elform=-1 and -2, respectively) were originally developed for performing highly 15. Simply Supported Square Plate: Transient Forced Vibration (thick shell mesh) Keywords: *CONTROL_IMPLICIT_AUTO *CONTROL_IMPLICIT_DYNAMICS *CONTROL_IMPLICIT_GENERAL *CONTROL_IMPLICIT_SOLVER *CONTROL_IMPLICIT_SOLUTION Description: A plate is subjected to a suddenly applied pressure on its top. A transient analysis is performed in order to obtain the response of the plate. Damping is present. On the lower surface, outer boundary nodes, ZU = . The finite element model is shown in Figure 15.1. Figure 15.1 – Finite element model with applied pressure on upper surface and Analysis Summary: Dim. Type Load Material Geometry Contact Solver Solution Method 3D Dynamic Pressure Damping Linear Linear - Implicit 1 - Linear Units: kg, m, s, N, Pa, N-m (kilogram, meter, second, Newton, Pascal, Newton-meter) Dimensional Data: Rectangular dimensions of square plate: 10.0 m x 10.0 m x 1.00 m. Material Data: Mass Density Young's Modulus Poisson's Ratio Damping ratio Load: Pressure Element Types: /kg m Pa 11 ρ= × 8.00 10 = × 2.00 10 ν = 0.3 %2=ζ = × 1.0 10 Pa S/R 2x2 IPI thick shell (elform=2) Assumed strain 2x2 IPI thick shell (elform=3) Assumed strain RI thick shell (elform=5) Material Models: *MAT_001 or *MAT_ELASTIC Damping: The damping factor d is easily found from the natural frequency of the system: id ωζ2= ) As the excited mode is the first, corresponding to (that from NAFEMS Benchmark Test FV52), we choose the damping factor relative to the first frequency: 288.380 45.897 rad s Hz ( / ω = = 1 11.535 = Hz Results Comparison: LS-DYNA X-direction bending stress, σxx , at (Node 161) on bottom surface plus its Z- displacement, ZU , are compared with NAFEMS Selected Benchmarks for Forced Vibration, Test 21T. Reference Condition - Center (Node 161) Peak Bending Stress σxx (Pa) Peak ZU (m) Steady-State ZU (m) NAFEMS Benchmark Test 21T 6.211 10× 4.524 10− × − 2.333 10− × − S/R 2x2 IPI thick shell (elform=2) 6.398 10× 4.937 10− × − 2.537 10− × − Assumed strain 2x2 IPI thick shell (elform=3) Assumed strain RI thick shell (elform=5) 6.350 10× 5.090 10− × − 2.616 10− × − 6.319 10× 5.022 10− × − 2.557 10− × − These nodal displacement results were generated by *DATABASE_NODOUT keyword while the axial stress (nodal) results were generated by *DATABASE_ELOUT (elout file) and *DATABASE_EXTENT_BINARY (eloutdet file provides detailed element output at integration points and connectivity nodes) keyword entries. You can set intout=stress or intout=all (*DATABASE_EXTENT_BINARY) and have stresses output file called eloutdet integration points (*DATABASE_ELOUT governs the output interval and *DATABASE_HISTORY_ TSHELL governs which elements are output). Setting nodout=stress or nodout=all in *DATABASE_EXTENT_BINARY will write the extrapolated nodal stresses to eloutdet. for all to a the LS-DYNA stress and strain output corresponds to integration point locations. Stress at a node is an artifact of the post-processor and represents an average of the surrounding integration point stresses (the value will likely be different with different post- Lobatto integration (intgrd=1 - *CONTROL_SHELL) was employed since it has an advantage in that the inner and outer integration points are on the shell surfaces. Gauss integration is the default through thickness integration rule (the default number of through thickness integration points is nip=2 - *SECTION_TSHELL) in LS-DYNA, where 1-10 integration points may be specified, whereas, with Lobatto integration, 3-10 integration points may be specified (for 2 point integration, the Lobatto rule is very inaccurate). The selectively reduced 2x2 IPI thick shell (elform=2), the assumed strain 2x2 IPI thick shell (elform=3), and the assumed strain RI thick shell (elform=5) all provide similar results for this transient forced vibration example, though slightly less stiff in comparison, both in stress and displacement. Remember that (a) only the higher order, selectively reduced 2x2 IPI thick shell (elform=2) provides a reasonable stress comparison for a single element through the thickness, although with a comparatively stiff result, and (b) the higher order, assumed strain 2x2 IPI thick shell (elform=3) and assumed strain RI thick shell (elform=5) formulations do provide acceptable results with at least two elements through the thickness (recommended) to capture the bending response. For this transient forced vibration example, with an element aspect ratio of 3.75, it is seen that the thick shell formulations, on the whole, compare better than the solid element formulation results. The exception to this would be the displacement comparison provided by the higher order, fully integrated S/R solid (both so-called efficient and accurate formulation choices) intended to address poor aspect ratios (elform=-1 and -2, respectively). For the selectively reduced 2x2 IPI thick shell (elform=2), the contour plot of the X- direction bending stress (Figure 15.2) and the Z-displacement (Figure 15.3) were obtained from the d3plot file at peak displacement time which were generated by the Figure 15.2 – Contour plot of the X-stress (elform=2) at peak displacement time. *TITLE Simply Supported Square Plate: Transient Forced Vibration (thick shell mesh) *CONTROL_IMPLICIT_AUTO $# iauto iteopt itewin dtmin dtmax dtexp kfail kcycle 0 11 5 0.0 0.0 *CONTROL_IMPLICIT_DYNAMICS $# imass gamma beta 1 0.500000 0.250000 *CONTROL_IMPLICIT_GENERAL $# imflag dt0 imform nsbs igs cnstn form zero_v 1 0.000100 2 1 2 *CONTROL_IMPLICIT_SOLVER $# lsolvr lprint negev order drcm drcprm autospc autotol 4 2 2 0 1 0.0 1 0.0 $# lcpack 2 *CONTROL_IMPLICIT_SOLUTION $# nsolvr ilimit maxref dctol ectol rctol lstol abstol 2 11 15 0.0010 0.0100 1.00e+10 0.900000 1.000000 $# dnorm diverg istif nlprint 2 1 1 2 $# arcctl arcdir arclen arcmth arcdmp 0 1 0.0 1 2 *CONTROL_SHELL $# wrpang esort irnxx istupd theory bwc miter proj 20.00000 0 0 0 2 2 1 $# rotascl intgrd lamsht cstyp6 tshell nfail1 nfail4 0.0 1 *CONTROL_TERMINATION $# endtim endcyc dtmin endeng endmas 0.020000 0 0.0 0.0 0.0 *DATABASE_ELOUT $# dt binary lcur ioopt 1.0000e-06 1 *DATABASE_NODFOR $# dt binary lcur ioopt 1.0000e-06 1 *DATABASE_NODOUT $# dt binary lcur ioopt 1.0000e-06 1 *DATABASE_BINARY_D3PLOT $# dt/cycl 0.001000 *DATABASE_EXTENT_BINARY $# neiph neips maxint strflg sigflg epsflg rtflg engflg $# cmpflg ieverp beamip dcomp shge stssz n3thdt ialemat $# nintsld pkp_sen sclp hydro msscl therm intout nodout 8 1.0 stress stress *DATABASE_HISTORY_TSHELL $# id1 id2 id3 id4 id5 id6 id7 id8 28 29 36 37 *DATABASE_NODAL_FORCE_GROUP $# nsid cid 164 *DATABASE_HISTORY_NODE $# nid1 nid2 nid3 nid4 nid5 nid6 nid7 nid8 161 164 *SET_NODE_LIST $# sid da1 da2 da3 da4 solver 164 0.0 0.0 0.0 0.0 $# nid1 nid2 nid3 nid4 nid5 nid6 nid7 nid8 164 *DAMPING_GLOBAL $# lcid valdmp stx sty stz srx sry srz 1 0 0.0 0.0 0.0 0.0 $# a1 o1 0.0 1.0000000e+06 0.10000000 1.0000000e+06 *ELEMENT_TSHELL $# eid pid n1 n2 n3 n4 n5 n6 n7 n8 1 1 1 37 41 5 2 38 42 6 192 1 283 319 323 287 284 320 324 288 *NODE $# nid x y z tc rc 1 0.0 0.0 0.0 3 324 10.00000000 10.00000000 1.00000000 *BOUNDARY_SPC_SET $#nid/nsid cid dofx dofy dofz dofrx dofry dofrz 1 0 0 0 1 *PART $# title material type # 1 (Elastic) $# pid secid mid eosid hgid grav adpopt tmid 1 1 1 *SECTION_TSHELL $# secid elform shrf nip propt qr/irid icomp tshear 1 2 0.0 5 0 0.0 $ 1 3 0.0 5 0 0.0 $ 1 5 0.0 5 0 0.0 *MAT_ELASTIC $# mid ro e pr da db not used 1 8000.0002.0000e+11 0.300000 0.0 0.0 0.0 *LOAD_SEGMENT $# lcid sf at n1 n2 n3 n4 1 1.000000 0.0 4 40 44 8 1 1.000000 0.0 284 320 324 288 *SET_NODE_LIST $# sid da1 da2 da3 da4 solver 1 0.0 0.0 0.0 0.0 $# nid1 nid2 nid3 nid4 nid5 nid6 nid7 nid8 1 37 73 109 145 181 217 253 289 293 297 301 305 309 313 317 321 285 249 213 177 141 105 69 33 29 25 21 17 13 9 5 *END 16. Transient Response of a Cylindrical Disk Impacting a Deformable Surface Keywords: *CONTROL_IMPLICIT_DYNAMICS *CONTROL_IMPLICIT_AUTO *CONTROL_IMPLICIT_GENERAL *CONTROL_IMPLICIT_SOLVER *CONTROL_IMPLICIT_SOLUTION *CONTACT_2D_AUTOMATIC_NODE_TO_SURFACE Description: A rigid cylindrical disk of given mass (m) is released from 1.0 inch height (h) and, accelerated by gravity (g), hits a deformable surface of given stiffness (k). Plot the velocity, displacement, and kinetic energy of the disk, plus identify the time of impact. The maximum displacement of the cylindrical disk is also to be determined. This simulation (Figure 16.1) is 2D plane strain (a choice of the available LS-DYNA options to address the impact - with the objects being rigid, this can be seen to negate the need for any planar type definition). The cylindrical disk is modeled with shell elements, x-y plane, which do not need additional constraints to ensure in-plane behavior. The deformable surface is modeled with rigid beam elements, x-y plane, to address contact, and a 1D translational spring element of a finite length (l), x-y plane, to address the deformation. As a geometric convenience, LS-DYNA employs the *SECTION_SHELL and *ELEMENT_SHELL entries to describe 2D plane stress, plane strain, and axisymmetric solids, and the *SECTION_BEAM and *ELEMENT_BEAM entries to describe 2D axisymmetric shells, and 2D plane strain beam elements. for suitable contact algorithm A the *CONTACT_2D_ AUTOMATIC_NODE_TO_SURFACE. For this algorithm, the contact stiffness is activated when a node nears a segment at some given tolerance. The stiffness is increased as the node moves closer with the full stiffness being used when the nodal point finally makes contact. Understanding LS-DYNA contact considerations adds to the focus of this example. A plot of the contact force history is sought. this problem Figure 16.1 – Finite element model with selected parts, elements, and nodes identified. Analysis Summary: Dim. Type Load Material Geometry Contact Solver 2D Dynamic Gravity Linear Linear 2D Implicit Solution Method 2-Nonlinear w/BFGS Units: lbf-s2/in, in, s, lbf, psi, lbf-in (blob, inch, second, pound force, pound force/inch2, pound force-inch) Dimensional Data: = × 1.0 10 in , = × 1.0 10 Material Data: Mass Density Nodal Mass ρ= = 3.995281 10 × 0.50 lbf − / in lbf − / in Spring Stiffness = 1.97392 10 × lb in / Load: Body Force Element Types: = = = = 0.0 in s / 0.0 in s / × 3.86 10 × 3.86 10 varied linearly to 3.86 10 × in s / , then held constant , = 0.0 / in s in s / , , = = × 1.0 10 × 1.0 10 s− 2D plane strain shell element (xy plane) - *SECTION_BEAM entry (elform=7) Plane strain (x-y plane) - *SECTION_SHELL entry - (elform=13) Translational spring - (SECTION_DISCRETE (dro=0) Material Models: *MAT_001 or *MAT_ELASTIC *MAT_020 or *MAT_RIGID Results Comparison: LS-DYNA results for velocity YV and displacement (plus the time) and maximum displacement of the cylindrical disk with W.T. Thomson's studies in Vibration Theory and Applications, 1965 (pg. 110). YU of the cylindrical disk at impact , are compared YmaxU Impact Time (s) Velocity YV (in/s) Displacement YU (in) Max. Disp. (in) YmaxU 0.07198 -27.7900 -1.0000 -1.5506 0.07240 -27.7728 -0.9978 -1.5524 Thomson [1965] Cylindrical LS-DYNA results are reported at the closet time point for the displacement value = − designated as full stiffness contact (i.e. 1.0000 in). YU The nodal results were generated by *DATABASE_NODOUT keyword, the kinetic energy by *DATABASE_MATSUM keyword, and the contact force by *DATABASE_ RCFORC keyword. Figure 16.2 provides the velocity history, and Figure 16.4 the kinetic energy history, all of the cylindrical disk. YV history, Figure 16.3 the vertical displacement YU Figure 16.5 gives the contact force between the cylindrical disk (slave) and the flexible surface (master). Figure 16.3 – Vertical displacement YU of the cylindrical disk. Figure 16.5 – Contact force between cylindrical disk (slave) and flexible surface (master). Input deck: *KEYWORD *TITLE Transient Response of a Cylindrical Disk Impacting a Flexible Surface *CONTROL_IMPLICIT_DYNAMICS $# imass gamma beta 1 0.500000 0.250000 *CONTROL_IMPLICIT_AUTO $# iauto iteopt itewin dtmin dtmax 1 11 5 1.00e-06 1.00e-04 *CONTROL_IMPLICIT_GENERAL $# imflag dt0 imform nsbs igs cnstn form 1 0.000100 0 0 0 *CONTROL_IMPLICIT_SOLVER $# lsolvr prntflg negeig order drcm drcprm autospc aspctl 4 2 2 0 1 0 1 0 $# lcpack 2 *CONTROL_IMPLICIT_SOLUTION $# nsolvr ilimit maxref dctol ectol rctol lstol abstol 2 11 15 0.0010 0.0100 1.00e+10 0.900000 1.00e-10 $# dnorm diverg istif nlprint nlnorm d3itctl cpchk 2 1 1 2 $# arcctl arcdir arclen arcmth arcdmp 0 1 0.0 1 2 *CONTROL_TERMINATION $# endtim endcyc dtmin endeng endmas 0.1100 *DATABASE_GLSTAT $# dt binary 1.0000e-04 1 *DATABASE_RCFORC $# dt binary 1.0000e-04 1 *DATABASE_NODOUT $# dt binary 1.0000e-04 1 *DATABASE_BINARY_D3PLOT $# dt/cycl lcdt/nr beam npltc psetid 1.0000e-03 *DATABASE_HISTORY_NODE $# nid1 nid2 nid3 nid4 ni5 nid6 nid7 nid8 166 1001 *PART $# title rigid cylindrical disk $# pid secid mid eosid hgid grav adpopt tmid 1 1 1 *SECTION_SHELL $# secid elform shrf nip propt qr/irid icomp setyp 1 13 0 4 $# t1 t2 t3 t4 nloc marea 1.0000 1.0000 1.0000 1.0000 *MAT_RIGID $ mid ro e pr n couple m alias 1 3.9952831 3.00e+07 0.3000 0.0 0.0 0.0 0.0 $ cmo con1 con2 1.0000 6.0 7.0 $lco_or_a1 a2 a3 v1 v2 v3 0.0 0.0 0.0 0.0 0.0 0.0 *PART discrete spring - flexible surface $# pid secid mid eosid hgid grav adpopt tmid 2 2 2 *SECTION_DISCRETE $# secid dro kd v0 cl fd 2 0 0 0 0.0 0.0 $# cdl tdl 0.0 0.0 *MAT_SPRING_ELASTIC $# mid k 2 1973.9200 *PART rigid plane beam (wall) $# pid secid mid eosid hgid grav adpopt tmid 3 3 3 *SECTION_BEAM $# secid elform shrf qr/irid cst scoor nsm 3 7 1.0000 1.0000 0.0000 $ ts1 ts2 tt1 tt2 0.1000 0.1000 *MAT_RIGID $ mid ro e pr n couple m alias 3 1.00e-07 3.00e+07 0.3000 0.0 0.0 0.0 0.0 $ cmo con1 con2 1.0000 6.0 7.0 $lco_or_a1 a2 a3 v1 v2 v3 0.0 0.0 0.0 0.0 0.0 0.0 *ELEMENT_BEAM 1002 3 1003 1001 1003 3 1001 1004 *ELEMENT_DISCRETE $ eid pid n1 n2 vid s pf offset 1001 2 1001 1002 0 1.0 0 0.0 *ELEMENT_SHELL $# eid pid n1 n2 n3 n4 n5 n6 n7 n8 $# nid x y z tc rc 1 -0.14142136 0.05857864 0.0 521 0.16180338 0.31755710 0.0 1001 0.0 -1.050 0.0 6 7 1002 0.0 -2.050 0.0 7 7 1003 -0.5 -1.050 0.0 6 7 1004 0.5 -1.050 0.0 6 7 $ 1001 0.0 -1.0 0.0 6 7 $ 1002 0.0 -2.0 0.0 7 7 $ 1003 -0.5 -1.0 0.0 6 7 $ 1004 0.5 -1.0 0.0 6 7 *CONTACT_2D_AUTOMATIC_NODE_TO_SURFACE $# ssid msid sfact freq fs fd dc membs -2 -1 0.10 0 0 0 0 0 $# tbirth tdeath sos som nds ndm cof init 0 0 0 0 0 0 0 0 $# vc vdc ipf slide istiff tiedgap 2 $*CONTACT_2D_PENALTY $# ssid msid tbirth tdeath $ 2 1 $# ext_pas theta1 theta2 tol_ig pen toloff frcscl oneway $ 0.10 0.00010 *SET_NODE_LIST $# sid da1 da2 da3 da4 1 $# nid1 nid2 nid3 nid4 nid5 nid6 nid7 nid8 1003 1001 1004 *SET_NODE_LIST $# sid da1 da2 da3 da4 2 $# nid1 nid2 nid3 nid4 nid5 nid6 nid7 nid8 155 166 177 *LOAD_BODY_Y $ lcid sf lciddr xc yc zc cid 1 1.0 *DEFINE_CURVE $# lcid sdir sfa sfo offa offo dattyp 1 0 1.0000 1.0000 0.0 0.0 $# a1 o1 0.000 0.000 0.001 386.00 1.000 386.00 *END Notes: 1. From the LS-DYNA User's Manual: Note that the 2D and 3D element types must not be mixed, and different types of 2D elements, i.e. plane strain, plane stress, and axisymmetric, must not be used together. The discrete (spring) 1D element can be used with either 2D or 3D elements. 2. Consider the two surfaces comprising a contact. It is necessary to designate one as a slave surface and the other as a master surface. Nodal points defining the slave surface are called slave nodes, and similarly, nodes defining the master surface are called master nodes. Each slave-master surface combination is referred to as a contact surface. If one surface is more finely zoned, it should be defined as the slave 3. By default, the true thickness of 2D shell elements is taken into account for *CONTACT_2D _AUTOMATIC_SURFACE_TO_SURFACE and _AUTOMATIC_ NODE_TO_SURFACE contacts. The user can override the true thickness by using the sos and som parameters on the contact entry. input example: *CONTACT_2D_AUTOMATIC_NODE_TO_SURFACE $# ssid msid sfact freq fs fd dc membs -2 -1 0.10 0 0 0 0 0 $# tbirth tdeath sos som nds ndm cof init 0 0 0 0 0 0 0 0 $# vc vdc ipf slide istiff tiedgap 2 $ *SET_NODE_LIST $# sid da1 da2 da3 da4 1 $# nid1 nid2 nid3 nid4 nid5 nid6 nid7 nid8 1003 1001 1004 *SET_NODE_LIST $# sid da1 da2 da3 da4 2 $# nid1 nid2 nid3 nid4 nid5 nid6 nid7 nid8 155 166 177 $ *NODE $# nid x y z tc rc 1001 0.0 -1.050 0.0 6 7 1002 0.0 -2.050 0.0 7 7 1003 -0.5 -1.050 0.0 6 7 1004 0.5 -1.050 0.0 6 7 There is a stiffness control variable available, cof, which allows the full stiffness to be gradually applied as a node approaches a segment. The tolerance for the stiffness appears to be hardwired internally in the LS-DYNA software. cof offers only two options: on (cof=0 - LS-DYNA default) or off (cof=1); no tolerance adjusting. Using cof=0 activates the contact stiffness as a node approaches a segment at some unknown value; the stiffness is increased as the node moves closer with the full stiffness being used when the nodal point finally makes contact. Using cof=1 does not turn on any contact stiffness until the nodal point makes full stiffness contact. It is observed that the contact output force calculation (*DATABASE_RCFORC) is not made (delayed) until full stiffness contact is made for either cof option. For cof=1, the contact force is calculated without a delay (due to full stiffness being applied without the gradual increase), but is nosier (oscillatory) than the other solution cof=0, at least for this example problem. 4. If the older penalty contact algorithms are used, *CONTACT_2D _PENALTY and _PENALTY_ FRICTION, the slave-master distinction is irrelevant. These contacts use the mid-surface of the 2D shell elements; thus, the shell thickness is not taken into coordinates to achieve reasonable results, e.g., the arrival time of a dropped rigid sphere onto a 2D shell plate of a moderate thickness. input example: *CONTACT_2D_PENALTY $# ssid msid tbirth tdeath 2 1 $# ext_pas theta1 theta2 tol_ig pen toloff frcscl oneway 0.10 0.00010 155 166 177 $ *SET_NODE_LIST $# sid da1 da2 da3 da4 1 $# nid1 nid2 nid3 nid4 nid5 nid6 nid7 nid8 1003 1001 1004 *SET_NODE_LIST $# sid da1 da2 da3 da4 2 $# nid1 nid2 nid3 nid4 nid5 nid6 nid7 nid8 155 166 177 $ *NODE $# nid x y z tc rc 1001 0.0 -1.0 0.0 6 7 1002 0.0 -2.0 0.0 7 7 1003 -0.5 -1.0 0.0 6 7 1004 0.5 -1.0 0.0 6 7 There is an adjustable, stiffness control variable available, toloff, which allows the full stiffness to be gradually applied as a node approaches a segment. From the LS-DYNA User's Manual: toloff - Tolerance for stiffness activation for implicit solution only. The contact stiffness is activated when a node approaches a segment at a distance equal to the segment length multiplied by toloff. The stiffness is increased as the node moves closer with the full stiffness being applied when the nodal point finally makes contact. It is observed that the contact output force calculation (*DATABASE_RCFORC) is 17. Natural Frequency of a Linear Spring-Mass System Keywords: *CONTROL_TIMESTEP *ELEMENT_DISCRETE *ELEMENT_MASS *MAT_SPRING_ELASTIC Description: A mass (m) is attached to a linear spring, as shown in Figure 17.1. The mass is initially = − displaced from its equilibrium position and released. Determine the period of vibration τ. 1.0 in The spring is modeled by one discrete element (*ELEMENT_DISCRETE) using a linear elastic spring material (*MAT_S01/*MAT_SPRING_ELASTIC). The lumped mass is modeled by an *ELEMENT_MASS entry. Figure 17.1 – Sketch representing the model. Analysis Summary: Dim. Type Load Material Geometry Contact Solver Solution Method 3D Dynamic Initially Displace Linear Linear - Explicit Units: lbf-s2/in, in, s, lbf, psi, lbf-in (blob, inch, second, pound force, pound force/inch2, pound force-inch) Dimensional Data: = × 1.0 10 in Material Data: Nodal Mass Spring Stiffness Element Types: − = = × 2.588 10 in lbf 5.0 / lbf − / in Translational spring - *SECTION_DISCRETE (dro=0) Lumped mass (*ELEMENT_MASS entry) Material Models: *MAT_S01 or *MAT_SPRING_ELASTIC Results Comparison: LS-DYNA results for the period of vibration related to this linear spring-mass system are compared with S.P. Timoshenko and D.H. Young studies in Vibration Problems in Engineering, 1955 (pg. 1). Timoshenko and Young [1955] Linear spring-mass system Period of Vibration τ (s) 0.14295 0.14295 This nodal displacement result and the computer period of vibration was generated by Figure 17.2 – Node 1 displacement UY . *TITLE Natural Frequency of a Linear Spring-Mass System *CONTROL_TERMINATION $# endtim endcyc dtmin endeng endmas 0.150000 0 0.0 0.0 0.0 *CONTROL_TIMESTEP $# dtinit tssfac isdo tslimt dt2ms lctm erode ms1st 1.000e-04 1.000e-04 0 0.0 0.0 0 0 0 $# dt2msf dt2mslc imscl 0.0 0 0 *DATABASE_NODOUT $# dt binary 0.000100 *DATABASE_BINARY_D3PLOT $# dt/cycl lcdt/nr beam npltc psetid 0.001000 *DATABASE_HISTORY_NODE $# nid1 nid2 nid3 nid4 ni5 nid6 nid7 nid8 1 *PART $# title linear elastic spring $# pid secid mid eosid hgid grav adpopt tmid 1 1 1 *SECTION_DISCRETE $# secid dro kd v0 cl fd 1 0 0.0 0.0 0.0 0.0 $# cdl tdl 0.0 0.0 *MAT_SPRING_ELASTIC $# mid k 1 5.00 *ELEMENT_DISCRETE $# eid pid n1 n2 vid s pf offset 1 1 1 2 0 1.00000 0 1.00000 *ELEMENT_MASS $# eid id mass pid 2 1 0.00258800 3 2 0.00258800 *NODE $# nid x y z tc rc 1 0.0 0.0 0.0 2 0.0 1.00000000 0.0 *BOUNDARY_SPC_NODE $#nid/nsid cid dofx dofy dofz dofrx dofry dofrz 2 0 1 1 1 1 1 1 *END Notes: 1. As an alternative, it is possible to model the linear spring with a *BEAM_ELEMENT the option discrete) and *MAT_066/*MAT_ LINEAR_ELASTIC_ (with 2. For simulations with linear stiffness, one could use the following implicit entries and perform a simple eigenvalue analysis: *CONTROL_IMPLICIT_EIGENVALUE $# neig center lflag lftend rflag rhtend eigmth shfscl 3 11.000 0 -1.00e+29 0 1.00e+29 2 0.0 *CONTROL_IMPLICIT_GENERAL $# imflag dt0 imform nsbs igs cnstn form 6 1.00e-04 2 1 2 The period could be obtained directly from the eigout results file generated by the *CONTROL_IMPLICIT_EIGENVALUE keyword as shown here: Natural Frequency of a Linear Spring-Mass System r e s u l t s o f e i g e n v a l u e a n a l y s i s: |------ frequency -----| MODE EIGENVALUE RADIANS CYCLES PERIOD 1 4.547474E-12 2.132481E-06 3.393948E-07 2.946421E+06 2 5.456968E-12 2.336015E-06 3.717884E-07 2.689702E+06 18. Natural Frequency of a Nonlinear Spring-Mass System Keywords: *CONTROL_TIMESTEP *ELEMENT_DISCRETE *ELEMENT_MASS *MAT_SPRING_NONLINEAR_ELASTIC Description: A mass (m) is attached to a nonlinear spring: = − The mass is initially displaced Determine the period of vibration τ. 1.0 in = + δk , as shown in Figure 18.1. from its equilibrium position and released. The spring is modeled by one discrete element (*ELEMENT_DISCRETE) using a nonlinear (*MAT_S04/*MAT_SPRING_NONLINEAR_ ELASTIC). The lumped mass is modeled by an *ELEMENT_MASS entry. spring material elastic To input the data for the *MAT_S04/*MAT_SPRING_NONLINEAR_ELASTIC it is ( )δF : necessary to convert the stiffness-deflection curve , using a *DEFINE_CURVE entry. This curve is converted to eleven . = F k points of force-deflection points in the range to a force-deflection δ δ δ ]1,0[=δ ( )δk + = Analysis Summary: Dim. Type Load Material Geometry Contact Solver Solution Method 3D Dynamic Initially Displace Non- linear Linear - Explicit - Units: lbf-s2/in, in, s, lbf, psi, lbf-in (blob, inch, second, pound force, pound force/inch2, pound force-inch) Dimensional Data: = × 1.0 10 in Material Data: Nodal Mass Spring Stiffness = = Element Types: − × 2.588 10 δk , + lbf = − 2.0 / in lbf / in , = 4.0 lbf / in Translational spring - *SECTION_DISCRETE (dro=0) Lumped mass (*ELEMENT_MASS entry) Material Models: *MAT_S04 or *MAT_SPRING_NONLINEAR_ELASTIC Results Comparison: LS-DYNA results for the period of vibration related to this nonlinear spring-mass system are compared with S.P. Timoshenko and D.H. Young studies in Vibration Problems in Engineering, 1955 (pg. 141). Timoshenko and Young [1955] Nonlinear spring-mass system Period of Vibration τ (s) 0.14470 This nodal displacement result and the computer period of vibration was generated by *DATABASE_NODOUT keyword (also see Figures 18.2 and 18.3). Figure 18.2 – Node 1 displacement UY . *TITLE Natural Frequency of a Nonlinear Spring-Mass System *CONTROL_TERMINATION $# endtim endcyc dtmin endeng endmas 0.150000 0 0.0 0.0 0.0 *CONTROL_TIMESTEP $# dtinit tssfac isdo tslimt dt2ms lctm erode ms1st 1.000e-04 1.000e-04 0 0.0 0.0 0 0 0 $# dt2msf dt2mslc imscl 0.0 0 0 *DATABASE_NODOUT $# dt binary 0.000100 *DATABASE_BINARY_D3PLOT $# dt/cycl lcdt/nr beam npltc psetid 0.001000 *DATABASE_HISTORY_NODE $# nid1 nid2 nid3 nid4 ni5 nid6 nid7 nid8 1 *PART $# title nonlinear elastic spring $# pid secid mid eosid hgid grav adpopt tmid 1 1 1 *SECTION_DISCRETE $# secid dro kd v0 cl fd 1 0 0.0 0.0 0.0 0.0 $# cdl tdl 0.0 0.0 *MAT_SPRING_NONLINEAR_ELASTIC $# mid lcd lcr 1 1 *DEFINE_CURVE $# lcid sdir sfa sfo offa offo dattyp 1 0 1.000000 1.000000 0.0 0.0 $# a1 o1 0.00 0.0000 0.10 0.2040 0.20 0.4320 0.30 0.7080 0.40 1.0240 0.50 1.5000 0.60 2.0640 0.70 2.7720 0.80 3.6480 0.90 4.7160 1.00 6.0000 *ELEMENT_DISCRETE $# eid pid n1 n2 vid s pf offset 1 1 1 2 0 1.00000 0 1.00000 *ELEMENT_MASS $# eid id mass pid 2 1 0.00258800 3 2 0.00258800 *NODE $# nid x y z tc rc 1 0.0 0.0 0.0 2 0.0 1.00000000 0.0 *BOUNDARY_SPC_NODE $#nid/nsid cid dofx dofy dofz dofrx dofry dofrz 2 0 1 1 1 1 1 1 Notes: 1. A somewhat better comparison could be achieved with a more detailed representation of the nonlinear spring stiffness. 2. As an alternative, *BEAM_ELEMENT NONLINEAR_ELASTIC_DISCRETE_BEAM material behavior. the option discrete) is possible to model the nonlinear spring with a and *MAT_067/*MAT_ (with it 3. For simulations with linear stiffness, one would use the following implicit entries and perform a simple eigenvalue analysis: *CONTROL_IMPLICIT_EIGENVALUE $# neig center lflag lftend rflag rhtend eigmth shfscl 3 11.000 0 -1.00e+29 0 1.00e+29 2 0.0 *CONTROL_IMPLICIT_GENERAL $# imflag dt0 imform nsbs igs cnstn form 6 1.00e-04 2 1 2 The period could be obtained directly from the eigout results file generated by the *CONTROL_IMPLICIT_EIGENVALUE keyword as shown here: Natural Frequency of a Nonlinear Spring-Mass System r e s u l t s o f e i g e n v a l u e a n a l y s i s: |------ frequency -----| MODE EIGENVALUE RADIANS CYCLES PERIOD 1 -9.094947E-11 9.536743E-06 1.517820E-06 6.588397E+05 2 4.547474E-12 2.132481E-06 3.393948E-07 2.946421E+06 3 4.961360E+03 7.043692E+01 1.121038E+01 8.920301E-02 However, for this example, the spring stiffness is nonlinear, represented by a piecewise linear curve. LS-DYNA will make a stiffness, from two force- displacement pairs, to compute an eigenvalue. Which pairs used will depend on whether there is an initial offset or not (provided via *ELEMENT_DISCRETE). If there is zero initial offset, the first two force-displacement pairs are used; if there is an initial offset, the two pairs on either side of the offset would be used; if the offset and displacement value are equal, LS-DYNA uses this as the upper pair. Using this stiffness value will not yield a correct period of vibration. 19. Buckling of a Axially Loaded Thin Walled Cylinder Keywords: *CONTROL_IMPLICIT_GENERAL *CONTROL_IMPLICIT_SOLUTION *CONTROL_IMPLICIT_BUCKLE *CONTROL_IMPLICIT_EIGENVALUE Description: A cylinder is loaded with a uniform distributed (equal value to each node) line load of P 1000 (compressive) along the top edge. Determine the critical buckling load. lbs = The lower end of the cylinder is clamped, i.e. fixed for all translational and rotational = , the upper end of the cylinder is only = 0=z directions ( = ). fixed in x and y direction ( = = z = : = U= : = The finite element model is shown in Figure 19.1. Figure 19.1 – Finite element model with applied axial load and boundary nodes Analysis Type: Dim. Type Load Material Geometry Contact Solver 3D Static Force Linear Linear - Implicit Solution Method 2-Nonlinear w/BFGS Units: lbf-s2/in, in, s, lbf, psi, lbf-in (blob, inch, second, pound force, pound force/inch2, pound force-inch) Dimensional Data: = × 1.20 10 in , cr = × 4.8 10 in , = × 1.0 10 in− Material Data: Mass Density Young's Modulus Poisson's Ratio = = ν = Load: − lbf − / in lbf / in × 1.00 10 × 1.00 10 0.3 Axial Load = × 1.00 10 lbs Element Types: Belytschko-Tsay shell (elform=2) S/R Hughes-Liu shell (elform=6) Belytschko-Wong-Chiang shell (elform=10) Fully integrated shell (elform=16) Material Models: *MAT_001 or *MAT_ELASTIC Results Comparison: LS-DYNA results for the critical buckling load of a thin walled cylinder under axial compression are compared with S.P. Timoshenko and J.M. Gere studies in Theory of Critical Buckling Load crP (lbf) Critical Axial σ (psi) Stress cr Timoshenko and Gere [1961] 3.8025 10× 1.2608 10× Belytschko-Tsay shell (elform=2) 3.8763 10× 1.2853 10× S/R Hughes-Liu shell (elform=6) 4.6226 10× 1.5327 10× Belytschko-Wong-Chiang shell (elform=10) 3.8763 10× 1.2853 10× Fully integrated shell (elform=16) 4.6086 10× 1.5281 10× The analytical solution for this problem, from Timoshenko and Gere [1961], is: * cr = ( 3 1 − ) = 1.2608 10 × psi with a mode shape that is sinusoidal both axially and circumferentially. The LS-DYNA critical load axial load: crP is computed from the first eigenvalue and the applied crP λ= = 3.8762 10 × × 1.0000 10 × lbf = 3.8762 10 × lbf while the critical axial stress crσ is given by cr = cr = 3.8763 10 3.0159 10 × × lbf in = 1.2853 10 × psi This result, for the one point quadrature shell elements (elform=2 and elform=10), is in good agreement with the analytical solution. The critical load and axial stress for the fully integrated shell elements (elform=6 and elform=16) is greater than the one point quadrature shell elements. The difference is not Eigenvalue Results: From the eigout file, generated by the *CONTROL_IMPLICIT_BUCKLE keyword: Belytschko-Tsay shell (elform=2): Buckling of a Thin Walled Cylinder Under Compression r e s u l t s o f e i g e n v a l u e a n a l y s i s: |------ frequency -----| MODE EIGENVALUE RADIANS CYCLES PERIOD 1 3.876317E+02 2 3.882852E+02 3 3.882852E+02 S/R Hughes-Liu shell (elform=6) Buckling of a Thin Walled Cylinder Under Compression r e s u l t s o f e i g e n v a l u e a n a l y s i s: |------ frequency -----| MODE EIGENVALUE RADIANS CYCLES PERIOD 1 4.622332E+02 2 4.622523E+02 3 4.700114E+02 Belytschko-Wong-Chiang shell (elform=10) Buckling of a Thin Walled Cylinder Under Compression r e s u l t s o f e i g e n v a l u e a n a l y s i s: |------ frequency -----| MODE EIGENVALUE RADIANS CYCLES PERIOD 1 3.876317E+02 2 3.882852E+02 3 3.882852E+02 Fully integrated shell (elform=16) Buckling of a Thin Walled Cylinder Under Compression r e s u l t s o f e i g e n v a l u e a n a l y s i s: |------ frequency -----| MODE EIGENVALUE RADIANS CYCLES PERIOD 1 4.608551E+02 2 4.608564E+02 3 4.681777E+02 The one point quadrature shell elements (elform =2 and elform=10) only provide the axial sinusoidal mode shape (10 half sine waves) as can be seen in Figure 19.2. The fully integrated shell elements (elform=6 and elform=16) provide both the axial and circumferential sinusoidal mode shapes (2 half sine waves axially and 20 half sine waves circumferentially) as can be seen in Figure 19.3. The eigenmodes for the one point quadrature elements and the fully integrated shell Figure 19.2 – First eigenmode with the 1000 lbf load applied (elform=10). *TITLE Buckling of a Thin Walled Cylinder Under Compression *CONTROL_IMPLICIT_GENERAL $# imflag dt0 imform nsbs igs cnstn form 1 0.100000 2 1 2 *CONTROL_IMPLICIT_SOLUTION $# nsolvr ilimit maxref dctol ectol not used lstol rssf 2 11 15 0.001000 0.010000 0.0 0.900000 1.000000 $# dnorm diverg istif nlprint 2 1 1 2 $# arcctl arcdir arclen arcmth arcdmp 0 1 0.0 1 2 *CONTROL_IMPLICIT_BUCKLE $# nmode 3 *CONTROL_IMPLICIT_EIGENVALUE $# neig center lflag lftend rflag rhtend eigmth shfscl 300.0 *CONTROL_TERMINATION $# endtim endcyc dtmin endeng endmas 1.000000 0 0.0 0.0 0.0 *CONTROL_SHELL $# wrpang esort irnxx istupd theory bwc miter proj 20.00000 0 0 0 2 1 1 1 $# rotascl intgrd lamsht cstyp6 tshell nfail1 nfail4 0.0 0 *DATABASE_BINARY_D3PLOT $# dt/cycl 0.010000 *PART $# title material type # 1 (Elastic) $# pid secid mid eosid hgid grav adpopt tmid 1 1 1 0 1 *SECTION_SHELL $# secid elform shrf nip propt qr/irid icomp setyp 1 2 0.0 0 1 0.0 0 1 $ 1 6 0.0 0 1 0.0 0 1 $ 1 10 0.0 0 1 0.0 0 1 $ 1 16 0.0 0 1 0.0 0 1 $# t1 t2 t3 t4 nloc marea 0.100000 0.100000 0.100000 0.100000 0 0.0 *MAT_ELASTIC $# mid ro e pr da db not used 1 0.0100001.0000e+07 0.300000 0.0 0.0 0.0 *HOURGLASS $# hgid ihq qm ibq q1 q2 qb qw 1 4 0.0 0 0.0 0.0 0.0 0.0 *SET_NODE_LIST_TITLE bottom nodes $# sid da1 da2 da3 da4 solver 1 0.0 0.0 0.0 0.0 $# nid1 nid2 nid3 nod4 nid5 nid6 nid7 nid8 1 2 3 4 5 6 7 8 9 10 11 12 13 14 15 16 17 18 19 20 21 22 23 24 25 26 27 28 29 30 31 32 33 34 35 36 37 38 39 40 41 42 43 44 45 46 47 48 49 50 51 52 53 54 55 56 57 58 59 60 61 62 63 64 65 66 67 68 69 70 71 72 73 74 75 76 0 0 0 0 *SET_NODE_LIST_TITLE top nodes $# sid da1 da2 da3 da4 solver $# nid1 nid2 nid3 nod4 nid5 nid6 nid7 nid8 2205 2206 2207 2208 2209 2210 2211 2212 2213 2214 2215 2216 2217 2218 2219 2220 2221 2222 2223 2224 2225 2226 2227 2228 2229 2230 2231 2232 2233 2234 2235 2236 2237 2238 2239 2240 2241 2242 2243 2244 2245 2246 2247 2248 2249 2250 2251 2252 2253 2254 2255 2256 2257 2258 2259 2260 2261 2262 2263 2264 2265 2266 2267 2268 2269 2270 2271 2272 2273 2274 2275 2276 2277 2278 2279 2280 0 0 0 0 *BOUNDARY_SPC_SET $#nid/nsid cid dofx dofy dofz dofrx dofry dofrz 1 0 1 1 1 1 1 1 *BOUNDARY_SPC_SET $#nid/nsid cid dofx dofy dofz dofrx dofry dofrz 2 0 1 1 0 0 0 0 *DEFINE_CURVE $# lcid sdir sfa sfo offa offo dattyp 1 0 0.0 0.0 0.0 0.0 $# a1 o1 0.0 0.0 1.00000000 13.15789474 *LOAD_NODE_SET $# nsid dof lcid sf cid m1 m2 m3 2 3 1 -1.000000 *ELEMENT_SHELL $# eid pid n1 n2 n3 n4 n5 n6 n7 n8 1 1 1 2 78 77 0 0 0 0 2204 1 2204 2129 2205 2280 0 0 0 0 *NODE $# nid x y z tc rc 1 0.000 48.000000 0.000 0 0 2280 3.963804 47.836056 120.00000 0 0 *END Notes: 1. The keyword entry *CONTROL_IMPLICIT_BUCKLE allows for buckling analysis at the end of the static implicit simulation. 2. The fully integrated and one point quadrature shell elements are formulated for nonlinear analysis. Although this analysis is linear, it was solved with a nonlinear Mesh Convergence Study: Seven different mesh refinements were studied for this simulation: original mesh 29 axial by 76 circumferential elements (Figure 19.4a) • by 3.9671 10 4.1379 10 in in × × 1st mesh refinement 58 axial by 152 circumferential elements × • by 1.9840 10 2.0690 10 in in × 2nd mesh refinement 87 axial by 228 circumferential elements (Figure 19.4b) • by 1.3227 10 1.3793 10 in in × × 3rd mesh refinement 116 axial by 304 circumferential elements • by 0.9921 10 1.0345 10 in in × × 4th mesh refinement 145 axial by 380 circumferential elements (Figure 19.4c) • by 0.7937 10 0.8276 10 in in × × 5th mesh refinement 174 axial by 456 circumferential elements × • by 0.6614 10 0.6897 10 in in × 6th mesh refinement 203 axial by 532 circumferential elements • by 0.5669 10 0.5911 10 in in × × Figure 19.4a - Finite element model for the original mesh Figure 19.4b - Finite element model for the 2nd mesh refinement (87 axial by 228 circumferential) discretization with applied axial load. Figure 19.4c - Finite element model for the 4th mesh refinement Mesh Convergence Results Comparison: LS-DYNA results for the critical buckling load of a thin walled cylinder under axial compression are compared for seven different mesh discretizations. analytical solution - 3.8025 10× lbf Belytschko-Wong- Chiang (elform=10) fully integrated shell (elform=16) original mesh (29 axial by 76 circumferential elements) 3.8763 10× 4.6086 10× 1st mesh refinement (58 axial by 152 circumferential elements) 3.8115 10× 4.0616 10× 2nd mesh refinement (87 axial by 228 circumferential elements) 3.8052 10× 3.9313 10× 3rd mesh refinement (116 axial by 304 circumferential elements) 3.8033 10× 3.8758 10× 4th mesh refinement (145 axial by 380 circumferential elements) 3.8026 10× 3.8480 10× 5th mesh refinement (174 axial by 456 circumferential elements) 3.8022 10× 3.8312 10× 6th mesh refinement (203 axial by 532 circumferential elements) 3.8019 10× 3.8207 10× For the Belytschko-Wong-Chiang (one point quadrature) shell element (elform=10), the 29 axial by 76 circumferential element mesh (original) critical buckling load result was in good agreement with the analytical solution. This element/mesh converged rapidly. The 29 axial by 76 circumferential element mesh only differed by less than 2% from the analytical solution while the 203 axial by 532 circumferential element mesh differed by less than 0.02%. For the fully integrated shell element (elform=16), the 29 axial by 76 circumferential element mesh (original) critical buckling load result was greater (over 21%) than the analytical solution. It is not known why. Doubling the number of elements axially and circumferentially reduces the critical buckling by about 10%; however, still not in good agreement with the analytical solution, especially considering the level of mesh refinement. Two further mesh refinements (116 axial by 304 circumferential element elements) were required to reach a similar good agreement (the 2% difference) with the one point quadrature shell element (elform=10) and the original mesh discretization. The 203 axial by 532 circumferential element mesh refinement for the fully integrated shell The one point quadrature shell element (elform=10) only provides the axial sinusoidal mode shape (Figures 19.5a and 19.5b): • 10 half sine waves in 29 axial by 76 circumferential element mesh (original), • 13 half sine waves in 58 axial by 152 circumferential element mesh, • 14 half sine waves in 87 axial by 228 circumferential element mesh, • 15 half sine waves in 116 axial by 304 circumferential element mesh, • 15 half sine waves in 145 axial by 380 circumferential element mesh, • 16 half sine waves in 174 axial by 456 circumferential element mesh, • 16 half sine waves in 203 axial by 532 circumferential element mesh, estimated from the eigenmode figures. The number of half sine waves is the number of buckles. It is not known why this element formulation only provides the axial sinusoidal Figure 19.5a - First eigenmode with the 1000 lbf load applied for Figure 19.5b - First eigenmode with the 1000 lbf load applied for the six integrated shell element (elform=16) provides both The fully circumferential sinusoidal mode shapes (Figures 19.6a and 19.6b): • 2 half sine waves axially and 20 half sine waves circumferentially in 29 axial by 76 the axial and circumferential element mesh (original), • 3 half sine waves axially and 24 half sine waves circumferentially in 58 axial by 152 circumferential element mesh, • 4 half sine waves axially and 28 half sine waves circumferentially in 87 axial by 228 circumferential element mesh, • 5 half sine waves axially and 30 half sine waves circumferentially in 116 axial by 304 circumferential element mesh, • 6 half sine waves axially and 32 half sine waves circumferentially in 145 axial by 380 circumferential element mesh, • 6 half sine waves axially and 32 half sine waves circumferentially in 174 axial by 456 circumferential element mesh, • 7 half sine waves axially and 34 half sine waves circumferentially in 203 axial by 532 circumferential element mesh. Figure 19.6a - First eigenmode with the 1000 lbf load applied for Figure 19.6b - First eigenmode with the 1000 lbf load applied for the six Notes: 1. Solution problems may exist: • because LS-DYNA buckling solutions assume the first buckling mode will be around 1.0 and/or • if numerous eigenvalues are clustered around that smallest bucking frequencies. For the refined meshes, for this problem, it was necessary to override the internal heuristic for picking a starting point for Lanczos shift strategy, which is the initial Eigen frequency shift. In these cases, the user must specify the initial shift via the 20. Membrane with a Hot Spot Keywords: *LOAD_THERMAL_LOAD_CURVE *MAT_ELASTIC_PLASTIC_THERMAL Description: This benchmark analyzes the behavior of shell elements subjected to a thermal load. Two distinct regions are modeled: the central hot-spot region (radius equal to r), subjected to the thermal strain , and the rest of the plate, which is at constant temperature with . Due to symmetry, only ¼ of the plate (side lengths 2L and thickness t) is modeled (Figures 20.1a and 20.1b). Tαε = ε= 0.0 The material defining is *MAT_ELASTIC_PLASTIC_THERMAL (*MAT_004), sensitive to temperature changes. The rest of the plate is defined with material *MAT_ELASTIC (*MAT_001). the hot spot The temperature is uniformly applied to the whole model by means of the *LOAD_ THERMAL_LOAD_CURVE keyword. Determine the y-component of the stress tensor along the edge y=0, just outside the hot spot. A fine mesh is required in the region of interest. To possibly achieve better accuracy, the value at the integration point is considered Figure 20.1a - Finite element model (¼ symmetry) with selected nodes and dimensions identified. Figure 20.1b - Finite element model of hot spot (blue region) and refined Analysis Summary: Dim. Type Load Material Geometry Contact Solver Solution Method 3D Static Thermal Linear Linear - Implicit 1-Linear Units: ton ,mm, s, N, MPa, N-m, C millimeter, degree Centigrade) (tonne, millmeter, second, Newton, MegaPascal, Newton- Dimensional Data: = 10.0 mm , = 1.00 mm , = 1.00 mm Material Data: Young's Modulus Poisson's Ratio Linear Expansion Load: Thermal Element Types: MPa = ν = = × 1.00 10 0.3 × 1.00 10 − mm mm C / / = 0.0 varied linearly to 100 Fully integrated shell (elform=16) Material Models: *MAT_001 or *MAT_ELASTIC *MAT_004 or *MAT_ELASTIC_PLASTIC_THERMAL Results Comparison: LS-DYNA global stress NAFEMS Background to Benchmark, Test T1. Reference Condition - Point Just Outside Hot Spot (Node 18) Global Stress - σyy (MPa) NAFEMS Benchmark Test T1 Element 1148 (average value) First in-plane integration point (2x2 quadrature) - element 1148 Node 18 5.0000 10× 4.7528 10× 4.5476 10× 4.3974 10× YYσ results were generated from *DATABASE_ELOUT (elout file) The global stress and *DATABASE_EXTENT_BINARY (eloutdet file provides detailed element output at integration points and connectivity nodes) keyword entries. You can set intout=stress or intout=all (*DATABASE_EXTENT_BINARY) and have file called eloutdet integration points stresses output (*DATABASE_ELOUT governs the output interval and *DATABASE_HISTORY_ SHELL governs which elements are output). Setting nodout=stress or nodout=all all in *DATABASE_EXTENT_BINARY will write the extrapolated nodal stresses to eloutdet. for all to a the LS-DYNA stress and strain outputs correspond to integration point locations. Stress at a node is an artifact of the post-processor and represents an average of the surrounding integration point stresses (the value will likely be different with different postprocessors). Shell element stresses are reported at through-thickness integration points. The location of those integration points depends on the number of integration points and the type of integration rule used, e. g., Gaussian, Lobatto, trapezoidal, user-defined rule . Fully-integrated shell formulations have 4 in-plane integration points at each through-thickness location. For these formulations, the 4 values of each stress component are averaged before being written to elout (except for the case of linear analysis when nsolvr=1 in *CONTROL_IMPLICIT_SOLUTION, in which case all 4 stress components are written to elout). Shell element stresses can be shown in the global, element, or material coordinate system. By default, shell element stresses/strains written to d3plot are global; shell stresses/strains written to elout are in the element local coordinate system (except for the case of linear analysis when nsolvr=1 in *CONTROL_IMPLICIT_SOLUTION, in which case stresses are in the global system). Shell element stresses/strains from d3plot are converted by LS- Even with this fine mesh in the region of interest, the large gradient temperature profile YYσ along the line of symmetry. The makes it difficult to capture the global stress average global stress of the element (Figure 20.2) provides the best comparative value (~5% difference), a few percent better than the nearest element integration point (~9% difference) and the extrapolated nodal (~12% difference) results. Figure 20.2 -Contour plot of global stress σyy . Maximum value at element 1148. Input deck: *KEYWORD *TITLE Membrane with a Hot Spot *CONTROL_IMPLICIT_GENERAL $# imflag dt0 imform nsbs igs cnstn form zer0_v 1 0.100000 2 1 2 0 0 0 *CONTROL_IMPLICIT_SOLUTION $# nsolvr ilimit maxref dctol ectol rctol lstol abstol 1 11 15 0.001000 0.010000 1.0e+10 0.900000 1.000000 $# dnorm diverg istif nlprint nlnorm d3itcl cpchk 2 1 1 0 2 0 0 $# arcctl arcdir arclen arcmth arcdmp arcpsi arcalf arctim 0 0 0.0 1 2 0.0 0.0 0.0 *CONTROL_SHELL $# wrpang esort irnxx istupd theory bwc miter proj 20.00000 0 -1 0 16 2 1 0 $# rotascl intgrd lamsht cstyp6 tshell 1.000000 0 0 1 0 *CONTROL_TERMINATION $# endtim endcyc dtmin endeng endmas 1.000000 0 0.0 0.0 0.0 $# neiph neips maxint strflg sigflg epsflg rtflg engflg 0 0 4 1 1 1 1 1 $# cmpflg ieverp beamip dcomp shge stssz n3thdt ialemat $# nintsld pkp_sen sclp hydro msscl therm intout nodout 1 1.0 stress stress *DATABASE_ELOUT $# dt/cycl 0.100000 *DATABASE_HISTORY_SHELL $# eid1 eid2 eid3 eid4 ei5 eid6 eid7 eid8 1148 *DATABASE_GLSTAT $# dt/cycl 0.100000 *DATABASE_MATSUM $# dt/cycl 0.100000 *DATABASE_BINARY_D3PLOT $# dt/cycl 0.100000 *PART $# title Part 1 for Mat 1 and Elem Type 16 $# pid secid mid eosid hgid grav adpopt tmid 1 1 1 *SECTION_SHELL $# secid elform shrf nip propt qr/irid icomp setyp 1 16 0.830000 1 1 0.0 0 1 $# t1 t2 t3 t4 nloc marea 1.000000 1.000000 1.000000 1.000000 0 0.0 *MAT_ELASTIC $# mid ro e pr da db not used 1 1.0000e+05 0.300000 0.0 0.0 0.0 *PART $# title Part 2 for Mat 2 and Elem Type 16 $# pid secid mid eosid hgid grav adpopt tmid 2 2 2 *SECTION_SHELL $# secid elform shrf nip propt qr/irid icomp setyp 2 16 0.830000 1 1 0.0 0 1 $# t1 t2 t3 t4 nloc marea 1.000000 1.000000 1.000000 1.000000 0 0.0 *MAT_ELASTIC_PLASTIC_THERMAL $# mid ro 2 $# t1 t2 t3 t4 t5 t6 t7 t8 0.0 1000.000 0.0 0.0 0.0 0.0 0.0 0.0 $# e1 e2 e3 e4 e5 e6 e7 e8 1.000e+05 1.000e+05 0.0 0.0 0.0 0.0 0.0 0.0 $# pr1 pr2 pr3 pr4 pr5 pr6 pr7 pr8 0.300000 0.300000 0.0 0.0 0.0 0.0 0.0 0.0 $# alpha1 alpha2 alpha3 alpha4 alpha5 alpha6 alpha7 alpha8 1.000e-05 1.000e-05 0.0 0.0 0.0 0.0 0.0 0.0 $# sigy1 sigy2 sigy3 sigy4 sigy5 sigy6 sigy7 sigy8 0.0 0.0 0.0 0.0 0.0 0.0 0.0 0.0 $# etan1 etan2 etan3 etan4 etan5 etan6 etan7 etan8 0.0 0.0 0.0 0.0 0.0 0.0 0.0 0.0 *ELEMENT_SHELL $# eid pid n1 n2 n3 n4 n5 n6 n7 n8 1 2 344 368 441 345 1456 2 434 432 433 453 *NODE $# nid x y z tc rc 1 1.00000000 0.0 0.0 1541 2.98852444 7.92062616 0.0 *BOUNDARY_SPC_SET 3 0 0 1 1 1 1 1 4 0 1 0 1 1 1 1 5 0 1 1 1 1 1 1 6 0 0 0 1 1 1 0 *SET_NODE_LIST_TITLE xsymm $# sid da1 da2 da3 da4 solver 3 0.0 0.0 0.0 0.0 $# nid1 nid2 nid3 nid4 nid5 nid6 nid7 nid8 19 20 181 182 183 185 323 324 325 326 327 328 330 332 17 306 304 302 301 300 299 297 296 172 170 169 167 48 47 46 45 18 1 11 12 186 187 188 333 334 335 336 337 338 8 272 270 268 267 265 264 155 153 151 82 81 *SET_NODE_LIST_TITLE ysymm $# sid da1 da2 da3 da4 solver 4 0.0 0.0 0.0 0.0 $# nid1 nid2 nid3 nid4 nid5 nid6 nid7 nid8 36 83 84 147 150 154 257 258 261 262 269 271 316 315 312 311 308 307 177 175 173 38 37 33 89 90 91 130 135 137 140 221 224 231 232 235 236 239 242 65 282 279 278 277 276 275 274 273 160 158 157 156 68 67 66 61 *SET_NODE_LIST_TITLE xy $# sid da1 da2 da3 da4 solver 5 0.0 0.0 0.0 0.0 $# nid1 nid2 nid3 nid4 nid5 nid6 nid7 nid8 80 *SET_NODE_LIST_TITLE whole $# sid da1 da2 da3 da4 solver 6 0.0 0.0 0.0 0.0 $# nid1 nid2 nid3 nid4 nid5 nid6 nid7 nid8 1 2 3 4 5 6 7 8 1537 1538 1539 1540 1541 *LOAD_THERMAL_LOAD_CURVE $# lcid lciddr 1 0 *DEFINE_CURVE $# lcid sdir sfa sfo offa offo dattyp 1 0 1.000000 1.000000 0.0 0.0 $# a1 o1 0.0 0.0 1.00000000 100.0000000 *END Notes: 1. The fully integrated and one point quadrature shell elements are formulated for non- linear analysis. Although this analysis is linear, it could have been solved with a non- linear solution method (nsolvr=2) which provides some slightly different stress output options . This was done for this simulation and it was found to 21. 1D Heat Transfer with Radiation Keywords: *CONTROL_SOLUTION *CONTROL_THERMAL_SOLVER *CONTROL_THERMAL_NONLINEAR *CONTROL_THERMAL_TIMESTEP *BOUNDARY_TEMPERATURE_SET *BOUNDARY_RADIATION_SET *MAT_THERMAL_ISOTROPIC Description: A 0.10 m long bar ( zL ), with square 0.01 m ( yL ) cross-section (Figure at one end (node 21.1), radiates (steady state) to an ambient temperature of 300 . The bar 11). The other end (node 1) is maintained at constant temperature 1000 is perfectly insulated along its length. There is zero internal heat generation. xL ) x 0.01 m ( = = Find the temperature at node 33 (x=0.000 m, y=0.010 m, z=0.100 m). The bar is meshed with 40 elements: ten elements along the length and four elements in the cross section. Analysis Summary: Dim. Type Load Material Geometry Contact Solver 3D Steady State Thermal Linear Linear - Thermal Non-Linear Solution Method 3-Diagonal scaled conjugate gradient Units: kg, m, s, N, Pa, N-m, C degree Centigrade) - Joule (J) is a N-m, Watt (W) is a J/s, 1 (kilogram, meter, second, Newton, Pascal, Newton-meter, ∆ = ∆ 1C Dimensional Data: xL = 0.01 , yL = 0.01 , zL = 0.10 Material Data: Mass Density Heat Capacity Thermal Conductivity Emissivity ρ= pC = ε= × 7.850 10 = 4.600 10 × × 5.560 10 0.980 /kg m / J kg C W m C / Stefan-Boltzman = 5.670 10 × − /W m K Load: Thermal Convection Initial Temperature Element Types: = 1000.0 × = 7.500 10 = 300.0 (constant) W m C (all nodes) / Fully integrated S/R solid (elform=2) Material Models: Results Comparison: LS-DYNA bar temperature at x=0.000 m, y=0.010 m, z= 0.100 m (Node 33) is compared with NAFEMS Background to Benchmark, Test T2. Reference Condition - Point Along Bar 0.1 m (Node 33) from Hot End (Node 23) Temperature ( K ) NAFEMS Benchmark Test T2 Node 33 9.2700 10× 9.2700 10× The fully integrated selectively reduced solid element (elform=2) model (also see Figure 21.2) provides an exact temperature comparison for this coarse mesh. The problem is 1D, although solved in 3D. The results are, as expected, the same for all x-y planes along the Z-direction. *TITLE 1D Heat Transfer with Radiation *CONTROL_SOLUTION $# soln nlq isnan lcint 1 0 0 0 *CONTROL_THERMAL_SOLVER $# atype ptype solver cgtol gpt eqheat fwork sbc 0 1 3 1.00e-06 8 1.000000 1.0000005.6700e-08 *CONTROL_THERMAL_NONLINEAR $# refmax tol dcp 20 1.000e-06 0.500000 *CONTROL_THERMAL_TIMESTEP $# ts tip its tmin tmax dtemp tscp 1 0.500000 1.000e-04 1.000e-04 0.100000 1.000000 0.500000 *CONTROL_TERMINATION $# endtim endcyc dtmin endeng endmas 1.00000 0 0.0 0.0 0.0 *DATABASE_TPRINT $# dt binary lcur ioopt 1.000000 0 0 1 *DATABASE_HISTORY_NODE $# nid1 nid2 nid3 nid4 nid5 nid6 nid7 nid8 11 22 33 44 55 66 77 88 99 *DATABASE_BINARY_D3PLOT $# dt lcdt beam npltc psetid 1.000000 0 0 0 0 *PART $# title Part 1 for TMat 1 and Elem Type 2 $# pid secid mid eosid hgid grav adpopt tmid 1 1 0 0 0 0 0 1 *SECTION_SOLID $# secid elform aet 1 2 1 *MAT_THERMAL_ISOTROPIC $# tmid tro tgrlc tgmult 1 7850.000 0.0 0.0 $# hc tc 460.0000 55.6000 *BOUNDARY_TEMPERATURE_SET $# nsid lcid cmult loc 1 0 1000.000 0 *BOUNDARY_RADIATION_SET $# ssid type 2 1 $# flcid fmult tilcid timult loc 05.5566e-08 0 300.0000 0 *INITIAL_TEMPERATURE_SET $# nsid temp loc 3 300.0000 0 *SET_NODE_LIST_TITLE A $# sid da1 da2 da3 da4 1 0.0 0.0 0.0 0.0 $# nid1 nid2 nid3 nid4 nid5 nid6 nid7 nid8 1 12 23 34 45 56 67 78 89 *SET_SEGMENT_TITLE B $# sid da1 da2 da3 da4 2 0.000 0.000 0.000 0.000 $# n1 n2 n3 n4 a1 a2 a3 a4 55 22 11 44 0.000 0.000 0.000 0.000 66 33 22 55 0.000 0.000 0.000 0.000 88 55 44 77 0.000 0.000 0.000 0.000 $# sid da1 da2 da3 da4 3 0.0 0.0 0.0 0.0 $# nid1 nid2 nid3 nid4 nid5 nid6 nid7 nid8 1 2 3 4 5 6 7 8 9 10 11 12 13 14 15 16 17 18 19 20 21 22 23 24 25 26 27 28 29 30 31 32 33 34 35 36 37 38 39 40 41 42 43 44 45 46 47 48 49 50 51 52 53 54 55 56 57 58 59 60 61 62 63 64 65 66 67 68 69 70 71 72 73 74 75 76 77 78 79 80 81 82 83 84 85 86 87 88 89 90 91 92 93 94 95 96 97 98 99 *ELEMENT_SOLID $# eid pid n1 n2 n3 n4 n5 n6 n7 n8 1 1 1 34 45 12 2 35 46 13 40 1 54 87 98 65 55 88 99 66 *NODE $# nid x y z tc rc 1 0.0 0.0 0.0 99 0.01000000 0.01000000 0.10000000 *END Notes: 1. The problem must be flagged as nonlinear if any boundary condition parameter is a function of temperature. This includes a linear (i.e., straight line) relationship. 4T boundary Iterations are needed to obtain the correct solution. Radiation is a condition. 2. The *CONTROL_THERMAL_NONLINEAR keyword is optional. For example, the default values for remax (maximum number of iterations allowed per time step), tol (temperature convergence tolerance), and dcp (divergence control tolerance) will be used, if the nonlinear keyword is omitted, with ptype>0 on *CONTROL_ 22. 1D Transient Heat Transfer in a Bar Keywords: *CONTROL_SOLUTION *CONTROL_THERMAL_SOLVER *CONTROL_THERMAL_TIMESTEP *BOUNDARY_TEMPERATURE_SET *INITIAL_TEMPERATURE_SET *MAT_THERMAL_ISOTROPIC Description: A 0.1 m long bar ( yL ) cross-section (Figure 22.1), is subjected at one end (node 6) to a varying thermal with the following law: . The other end (node 1) is maintained at constant temperature zL ), with square 0.01 m ( xL ) x 0.01 m ( 100sin / 40 ( ) = C= . The bar is perfectly insulated along its length. Determine the temperature at 0.02 m from the hot end after 32 seconds. The bar is meshed with 20 elements: five elements along the length and four elements in the cross section. Analysis Summary: Dim. Type Load Material Geometry Contact Solver 3D Thermal Transient Thermal Linear Linear - Thermal Linear Solution Method 3-Diagonal scaled conjugate gradient Units: kg, m, s, N, Pa, N-m, C degree Centigrade) - Joule (J) is a N-m, Watt (W) is a J/s (kilogram, meter, second, Newton, Pascal, Newton-meter, Dimensional Data: xL = 0.01 , yL = 0.01 , zL = 0.10 Material Data: Mass Density Heat Capacity Thermal Conductivity ρ= pC × 7.200 10 = 4.405 10 × = 3.500 10 × /kg m / J kg C W m C / Load: Thermal Convection Initial Temperature Element Types: (constant) W m C / = 100 × = 7.500 10 C= (all nodes) Fully integrated S/R solid (elform=2) Material Models: Results Comparison: LS-DYNA bar temperature at x=0.0050 m, y=0.005 m, z= 0.080 m (Node 35) is compared with NAFEMS Background to Benchmark, Test T3. Reference Condition - Point Along Bar 0.2 m (Node 35) from Hot End (Node 36) Temperature ( C ) NAFEMS Benchmark Test T3 Node 35 3.6600 10× 3.4861 10× The fully integrated selectively reduced solid element (elform=2) model (Figure 22.2) provides a reasonable temperature comparison for this coarse mesh. The problem is 1D, although done in 3D. The results are, as expected, the same for all x-y planes along the Z-direction. Figure 22.2 -Contour plot of temperatures at time =32.0 seconds The histories of temperature for two nodes (35 and 36) used in the comparison are shown in Figure 22.3. Figure 22.3 - Temperature histories for nodes 35 and 56. Input deck: *KEYWORD *TITLE 1D Transient Heat Transfer in a Bar *CONTROL_SOLUTION $# soln nlq isnan lcint 1 0 0 0 *CONTROL_THERMAL_SOLVER $# atype ptype solver cgtol gpt eqheat fwork sbc 1 0 3 1.00e-06 8 1.000000 1.000000 0.0 *CONTROL_THERMAL_TIMESTEP $# ts tip its tmin tmax dtemp tscp 1 0.500000 1.000e-04 1.000e-04 0.100000 1.000000 0.500000 *CONTROL_TERMINATION $# endtim endcyc dtmin endeng endmas 32.00000 0 0.0 0.0 0.0 *DATABASE_TPRINT $# dt binary lcur ioopt 1.000000 0 0 1 *DATABASE_HISTORY_NODE $# nid1 nid2 nid3 nid4 nid5 nid6 nid7 nid8 5 6 11 12 17 18 23 24 29 30 35 36 41 42 47 48 53 54 *DATABASE_BINARY_D3PLOT $# dt lcdt beam npltc psetid 1.000000 0 0 0 0 *PART $# title $# pid secid mid eosid hgid grav adpopt tmid 1 1 0 0 0 0 0 1 *SECTION_SOLID $# secid elform aet 1 2 1 *MAT_THERMAL_ISOTROPIC $# tmid tro tgrlc tgmult 1 7200.000 0.0 0.0 $# hc tc 440.5000 35.0000 *BOUNDARY_TEMPERATURE_SET $# nsid lcid cmult loc 1 0 0.0 0 *BOUNDARY_TEMPERATURE_SET $# nsid lcid cmult loc 2 1 1.000000 0 *INITIAL_TEMPERATURE_SET $# nsid temp loc 3 0.0 0 *SET_NODE_LIST_TITLE A $# sid da1 da2 da3 da4 1 0.0 0.0 0.0 0.0 $# nid1 nid2 nid3 nid4 nid5 nid6 nid7 nid8 1 7 13 19 25 31 37 43 49 *SET_NODE_LIST_TITLE B $# sid da1 da2 da3 da4 2 0.0 0.0 0.0 0.0 $# nid1 nid2 nid3 nid4 nid5 nid6 nid7 nid8 6 12 18 24 30 36 42 48 54 *SET_NODE_LIST_TITLE central $# sid da1 da2 da3 da4 3 0.0 0.0 0.0 0.0 $# nid1 nid2 nid3 nid4 nid5 nid6 nid7 nid8 1 2 3 4 5 6 7 8 9 10 11 12 13 14 15 16 17 18 19 20 21 22 23 24 25 26 27 28 29 30 31 32 33 34 35 36 37 38 39 40 41 42 43 44 45 46 47 48 49 50 51 52 53 54 *DEFINE_CURVE $# lcid sdir sfa sfo offa offo dattyp 1 0 0.0 0.0 0.0 0.0 $# a1 o1 0.0 0.0 1.00000000 7.84194040 2.00000000 15.63558102 3.00000000 23.33292198 4.00000000 30.88655281 5.00000000 38.24995041 6.00000000 45.37776184 7.00000000 52.22608948 8.00000000 58.75275421 9.00000000 64.91754913 10.00000000 70.68251801 11.00000000 76.01214600 12.00000000 80.87360382 13.00000000 85.23696136 14.00000000 89.07533264 15.00000000 92.36508179 16.00000000 95.08594513 17.00000000 97.22116852 18.00000000 98.75759888 19.00000000 99.68576813 20.00000000 99.99996948 22.00000000 98.78250122 23.00000000 97.25833130 24.00000000 95.13513947 25.00000000 92.42600250 26.00000000 89.14760590 27.00000000 85.32013702 28.00000000 80.96717834 29.00000000 76.11553955 30.00000000 70.79508972 31.00000000 65.03861237 32.00000000 58.88155746 *ELEMENT_SOLID $# eid pid n1 n2 n3 n4 n5 n6 n7 n8 1 1 1 19 25 7 2 20 26 8 20 1 29 47 53 35 30 48 54 36 *NODE $# nid x y z tc rc 1 0.0 0.0 0.0 54 0.01000000 0.01000000 0.10000000 *END 23. 2D Heat Transfer with Convection Keywords: *CONTROL_SOLUTION *CONTROL_THERMAL_SOLVER *CONTROL_THERMAL_TIMESTEP *MAT_THERMAL_ISOTROPIC *BOUNDARY_CONVECTION_SET *BOUNDARY_TEMPERATURE_SET *INITIAL_TEMPERATURE_SET Description: = = xL yL 1.00 in depth) of rectangular cross-section ( A slab ( ) shown in Figure 23.1 is subjected to the following thermal loads for a steady state simulation: • constant Temperature 0 = • natural convection to the ambient temperature on the face defined by nodes 78-79-85-95, 0= nodes 12-85-79-18 and 1-12-18-2 (convection coefficient face defined by nodes 1-2-78-95 is adiabatically insulated. on the faces defined by W m C × 7.50 10 1.00 0.60 by 100 Ta zL ), = / • = Find the temperature at node 225 (x=0.60 m, y=1.00 m, z=-0.20 m). Analysis Summary: Dim. Type Load Material Geometry Contact Solver Thermal Linear Linear - Thermal 3D Steady State Units: Solution Method 3-Diagonal scaled conjugate gradient kg, m, s, N, Pa, N-m, C degree Centigrade) - Joule (J) is a N-m, Watt (W) is a J/s (kilogram, meter, second, Newton, Pascal, Newton-meter, Dimensional Data: xL = 0.60 , yL = 1.00 , zL = 1.00 Material Data: Mass Density Heat Capacity Thermal Conductivity ρ= pC = × 8.000 10 = 1.000 10 × 5.200 10 × /kg m / J kg C W m C / Load: Thermal Convection Element Types: = = 100 × 7.500 10 (constant) W m C / Fully integrated S/R solid (elform=2) Material Models: Results Comparison: LS-DYNA slab edge temperature at x=0.60 m, y=1.00 m, z=-0.20 m (Node 225) are compared with NAFEMS Background to Benchmark, Test T4. Reference Condition - Point Along Slab Edge (Node 225) Temperature ( C ) NAFEMS Benchmark Test T4 Node 225 1.8300 10× 1.7954 10× The fully integrated selectively reduced solid element (elform=2) model (Figure 23.2) provides a reasonable temperature comparison for this relatively coarse mesh. The problem is 2D, although solved in 3D. The results are, as expected, the same for all planes in the 3rd dimension (Y-direction in this case). *TITLE 2D Heat Transfer with Convection *CONTROL_SOLUTION $# soln nlq isnan lcint 1 0 0 0 *CONTROL_THERMAL_SOLVER $# atype ptype solver cgtol gpt eqheat fwork sbc 0 0 3 1.00e-06 8 1.000000 1.000000 0.000000 *CONTROL_TERMINATION $# endtim endcyc dtmin endeng endmas 1.000000 0 0.000 0.000 0.000 *DATABASE_TPRINT $# dt binary lcur ioopt 1.000000 0 0 1 *DATABASE_HISTORY_NODE $# nid1 nid2 nid3 nid4 nid5 nid6 nid7 nid8 225 171 371 372 373 374 375 376 377 378 379 *DATABASE_BINARY_D3PLOT $# dt lcdt beam npltc psetid 1.000000 0 0 0 0 *PART $# title Part 1 for Mat 1 and Elem Type 2 $# pid secid mid eosid hgid grav adpopt tmid 1 1 0 0 0 0 0 1 *SECTION_SOLID $# secid elform aet 1 2 0 *MAT_THERMAL_ISOTROPIC $# tmid tro tgrlc tgmult tlat hlat 1 8000.000 0.000 0.000 0.000 0.000 $# hc tc 1.000 52.0000 *BOUNDARY_CONVECTION_SET $# ssid 1 $# hlcid hmult tlcid tmult loc 0 750.00000 0 0.000 0 *BOUNDARY_CONVECTION_SET $# ssid 2 $# hlcid hmult tlcid tmult loc 0 750.00000 0 0.000 0 *BOUNDARY_TEMPERATURE_SET $# nsid lcid cmult loc 1 0 100.00000 0 *INITIAL_TEMPERATURE_SET $# nsid temp loc 1 100.00000 0 *SET_NODE_LIST_TITLE frontt100 $# sid da1 da2 da3 da4 1 0.000 0.000 0.000 0.000 $# nid1 nid2 nid3 nid4 nid5 nid6 nid7 nid8 78 79 80 81 82 83 84 85 86 87 88 89 90 91 92 93 94 95 96 97 98 99 100 101 102 103 104 105 106 107 108 109 110 111 112 113 114 115 116 117 118 119 120 121 122 123 124 125 126 127 128 129 130 131 132 133 134 135 136 137 138 139 140 141 142 143 144 145 146 147 148 149 150 151 152 153 154 0 0 0 *SET_SEGMENT_TITLE $# sid da1 da2 da3 da4 1 0.000 0.000 0.000 0.000 $# n1 n2 n3 n4 a1 a2 a3 a4 18 19 434 164 0.000 0.000 0.000 0.000 370 226 85 94 0.000 0.000 0.000 0.000 *SET_SEGMENT_TITLE backt0 $# sid da1 da2 da3 da4 2 0.000 0.000 0.000 0.000 $# n1 n2 n3 n4 a1 a2 a3 a4 2 11 33 28 0.000 0.000 0.000 0.000 77 13 12 27 0.000 0.000 0.000 0.000 *ELEMENT_SOLID $# eid pid n1 n2 n3 n4 n5 n6 n7 n8 1 1 2 28 33 11 163 213 443 289 600 1 847 370 226 272 154 94 85 96 *NODE $# nid x y z tc rc 1 0.000 1.0000000 -1.0000000 0 0 847 0.5000000 0.9000000 -0.1000000 0 0 *END Notes: 1. A two-dimensional model simulation could be made using the plane stress (x-y plane) element formulation (elform=12 given on *SECTION_SHELL keyword) with a constant temperature through the thickness. Under the keyword *CONTROL_ SHELL, the option tshell allows the user to choose between a constant temperature through the thickness and a 20 node brick formulation which allows heat conduction 24. 3D Thermal Load Keywords: *CONTROL_IMPLICIT_GENERAL *CONTROL_IMPLICIT_SOLUTION *LOAD_THERMAL_VARIABLE_NODE *MAT_ELASTIC_PLASTIC_THERMAL Description: The solid cylinder tapering to a sphere geometry depicted below (Figure 24.1) is subjected to a prescribed temperature gradient. Two analyses, one with a coarse mesh 5 x 1 x 3 and one with a fine mesh 10 x 2 x 3 (Figure 24.2), are made. The model represents ¼ of the total geometry. Symmetry conditions on the plane x-z and y-z are enforced. The faces parallel to the plane x-y are simply supported in the Z-direction. The linear temperature loading (radial and axial direction) (Figure 24.3) is applied by means of temperature dependent material with thermal expansion coefficient and resulting thermal strain Tαε = . Determine the stress in the Z-direction at Node A (Node 10 for the coarse-mesh model and Node 16 for the fine-mesh model). Figure 24.1 - Schematic of ¼ model and cross-section dimensions Figure 24.2 - Finite element models with selected node and element identified. Figure 24.3 - Finite element models with temperature loading. Analysis Summary: Dim. Type Load Material Geometry Contact Solver Solution Method 3D Static Thermal Linear Linear - Implicit 1-Linear Units: kg, m, s, N, Pa, N-m, C degree Centigrade) - Joule (J) is a N-m, Watt (W) is a J/s (kilogram, meter, second, Newton, Pascal, Newton-meter, Dimensional Data: Material Data: Young's Modulus Poisson's Ratio Linear Expansion Load: Thermal Element Types: 11 Pa = ν = = × 2.10 10 0.3 × 2.30 10 − m m C / / ( T C ) = + + Fully integrated S/R solid (elform=2) Material Models: *MAT_004 or *MAT_ELASTIC_PLASTIC_THERMAL Results Comparison: zzσ at inner point on yz-symmetry plane (coarse mesh - Node LS-DYNA global stress 10, Element 3: fine mesh - Node 16, Element 5) is compared with NAFEMS Background to Benchmarks, Test LE11. Reference Condition - Inner Point on Symmetry Plane Coarse Mesh - Global Stress - zzσ (MPa) Fine Mesh - Global zzσ (MPa) Stress - NAFEMS Benchmark Test LE11 Element 3 (coarse) - Element 5 (fine) - (an averaged value) First in-plane integration point - Elem 3 (coarse) - Element 5 (fine) Node 10 (coarse) - Node 16 (fine) − 1.0500 10 × − 1.0500 10 × − 6.1849 10 × − 7.5890 10 × − 7.9107 10 × − 8.5217 10 × − 9.2071 10 × − 9.2102 10 × zzσ results were generated from *DATABASE_ELOUT (elout file) and The global stress *DATABASE_EXTENT_BINARY (eloutdet file provides detailed element output at By default, stresses/strains for solids are written to d3plot and elout in the global coordinate system. The elout file contains only the values at the element centroid (average of 8 integration points). You can set intout=stress or intout=all (*DATABASE_EXTENT_BINARY) and have stresses output file called eloutdet integration points (*DATABASE_ELOUT governs the output interval and *DATABASE_HISTORY_ SOLID governs which elements are output). Setting nodout=stress or nodout=all in *DATABASE_EXTENT_BINARY will write the extrapolated nodal stresses to eloutdet. for all to a the LS-DYNA stress and strain outputs correspond to integration point locations. Stress at a node is an artifact of the post-processor and represents an average of the surrounding integration point stresses (the value will likely be different with different postprocessors). zzσ at Both meshes are rather coarse which makes it difficult to capture the global stress the inner point along yz-symmetry plane. The extrapolated nodal stress results (also see Figures 24.4 and 24.5) provide the best comparative value (~12% difference for both meshes), primarily due to the nodal location. As expected, the fine mesh does a better job of capturing the overall contouring. The average global stress of the element provides the least acceptable comparative value results (~40% and ~25% differences), again not unexpected, while the nearest element integration point results provided significant improvement (~25% and ~15% differences) due to the larger integration sample (8 points as compared to 1) and nodal location. Figure 24.4 - Coarse mesh contour plots of global stress σzz with average value given for Element 3. On the left is in-plane integration point contouring while on the right Figure 24.5 - Fine mesh contour plots of global stress σzz with average value given for Element 5. On the left is in-plane integration point contouring while on the right is extrapolated nodal stress contouring with specification values given at Node 16. Input deck: *KEYWORD *TITLE 3D Thermal Load (coarse mesh) *CONTROL_IMPLICIT_GENERAL $# imflag dt0 imform nsbs igs cnstn form 1 1.000000 2 1 2 *CONTROL_IMPLICIT_SOLUTION $# nsolvr ilimit maxref dctol ectol rctol lstol abstol 1 11 15 0.001000 0.010000 1.0e+10 0.900000 1.000000 $# dnorm diverg istif nlprint nlnorm d3itcl cpchk 2 1 1 2 2 0 0 $# arcctl arcdir arclen arcmth arcdmp arcpsi arcalf arctim 0 1 0.0 1 2 0.0 0.0 0.0 *CONTROL_TERMINATION $# endtim endcyc dtmin endeng endmas 1.000000 0 0.0 0.0 0.0 *DATABASE_EXTENT_BINARY $# neiph neips maxint strflg sigflg epsflg rtflg engflg 0 0 0 1 1 1 1 1 $# cmpflg ieverp beamip dcomp shge stssz n3thdt ialemat $# nintsld pkp_sen sclp hydro msscl therm intout nodout 8 1.0 stress stress *DATABASE_ELOUT $# dt/cycl 0.100000 *DATABASE_HISTORY_SOLID $# eid1 eid2 eid3 eid4 ei5 eid6 eid7 eid8 3 *DATABASE_BINARY_D3PLOT $# dt/cycl 1.000000 *PART $# title Part 1 for Mat 1 and Elem Type 2 $# pid secid mid eosid hgid grav adpopt tmid 1 1 1 *SECTION_SOLID $# secid elform aet 1 2 1 *MAT_ELASTIC_PLASTIC_THERMAL $# mid ro 1 1.000000 0.0 1000.000 0.0 0.0 0.0 0.0 0.0 0.0 $# e1 e2 e3 e4 e5 e6 e7 e8 2.100e+11 2.100e+11 0.0 0.0 0.0 0.0 0.0 0.0 $# pr1 pr2 pr3 pr4 pr5 pr6 pr7 pr8 0.300000 0.300000 0.0 0.0 0.0 0.0 0.0 0.0 $# alpha1 alpha2 alpha3 alpha4 alpha5 alpha6 alpha7 alpha8 2.300e-04 2.300e-04 0.0 0.0 0.0 0.0 0.0 0.0 $# sigy1 sigy2 sigy3 sigy4 sigy5 sigy6 sigy7 sigy8 0.0 0.0 0.0 0.0 0.0 0.0 0.0 0.0 $# etan1 etan2 etan3 etan4 etan5 etan6 etan7 etan8 0.0 0.0 0.0 0.0 0.0 0.0 0.0 0.0 *ELEMENT_SOLID $# eid pid n1 n2 n3 n4 n5 n6 n7 n8 1 1 1 13 16 4 2 14 17 5 15 1 35 39 40 36 43 47 48 44 *NODE $# nid x y z tc rc 1 1.0000000 0.000 0.000 0 0 48 0.000 1.0000000 1.7900000 0 0 *SET_NODE_LIST_TITLE base $# sid da1 da2 da3 da4 solver 1 0.0 0.0 0.0 0.0 $# nid1 nid2 nid3 nid4 nid5 nid6 nid7 nid8 19 7 4 16 *SET_NODE_LIST_TITLE top $# sid da1 da2 da3 da4 solver 2 0.0 0.0 0.0 0.0 $# nid1 nid2 nid3 nid4 nid5 nid6 nid7 nid8 43 47 46 42 *SET_NODE_LIST_TITLE xsymm $# sid da1 da2 da3 da4 solver 3 0.0 0.0 0.0 0.0 $# nid1 nid2 nid3 nid4 nid5 nid6 nid7 nid8 23 11 24 12 28 32 40 36 *SET_NODE_LIST_TITLE ysymm $# sid da1 da2 da3 da4 solver 4 0.0 0.0 0.0 0.0 $# nid1 nid2 nid3 nid4 nid5 nid6 nid7 nid8 2 14 3 15 25 29 33 37 *SET_NODE_LIST_TITLE z+ysymm $# sid da1 da2 da3 da4 solver 5 0.0 0.0 0.0 0.0 $# nid1 nid2 nid3 nid4 nid5 nid6 nid7 nid8 1 13 41 45 *SET_NODE_LIST_TITLE z+xsymm $# sid da1 da2 da3 da4 solver 6 0.0 0.0 0.0 0.0 $# nid1 nid2 nid3 nid4 nid5 nid6 nid7 nid8 22 10 48 44 *BOUNDARY_SPC_SET $#nid/nsid cid dofx dofy dofz dofrx dofry dofrz 1 0 0 0 1 *BOUNDARY_SPC_SET $#nid/nsid cid dofx dofy dofz dofrx dofry dofrz 2 0 0 0 1 *BOUNDARY_SPC_SET $#nid/nsid cid dofx dofy dofz dofrx dofry dofrz 3 0 1 0 0 *BOUNDARY_SPC_SET $#nid/nsid cid dofx dofy dofz dofrx dofry dofrz 4 0 0 1 0 *BOUNDARY_SPC_SET $#nid/nsid cid dofx dofy dofz dofrx dofry dofrz 6 0 1 0 1 *LOAD_THERMAL_VARIABLE_NODE $# nid ts tb lcid 1 1.000000 0.0 1 48 2.790000 0.0 1 *DEFINE_CURVE $# lcid sdir sfa sfo offa offo dattyp 1 0 0.0 0.0 0.0 0.0 $# a1 o1 0.0 1.00000000 1.00000000 1.00000000 *END Notes: 1. The fully integrated solid elements are formulated for nonlinear analysis. Although this analysis is linear, it could have been solved with a nonlinear solution method (nsolvr=2). This was done for this simulation and it was found to yield results with some differences (less than 0.01% for coarse mesh and ~4% for fine mesh) from the linear analysis (nsolvr=1). It is not understood why the fine mesh offers this difference. 2. Fully-integrated solid formulations have 8 in-volume integration points for each element. For these formulations, the 8 values of each stress component are averaged at the element centroid before being written to elout. 3. If setting nintsld=8 on *DATABASE_EXTENT_BINARY, LS-DYNA will write stresses at all integration points for solid elements (also given in eloutdet) to the d3plot file. When this option is set, LS-PrePost applies the stress values to the nodes from the closest integration point and after that, the average value from the contributions are computed and presented in the stress fringe plot. 4. A command line option (extrapolate 1) is added to LS-PrePost, which will linearly extrapolate the values from integration points to the nodes (the extrapolated nodal stresses are also given in eloutdet). 5. For elastic bending, two integrations points through the thickness is the minimum number. For plastic bending, three integrations points through the thickness is the 25. Cooling of a Billet via Radiation Keywords: *CONTROL_SOLUTION *CONTROL_THERMAL_SOLVER *CONTROL_THERMAL_NONLINEAR *CONTROL_THERMAL_TIMESTEP *BOUNDARY_TEMPERATURE_SET *BOUNDARY_RADIATION_SET *MAT_THERMAL_ISOTROPIC Description: = = ft 4.00 2.00 A billet ( zL ) shown in Figure 25.1 is initially at temperature ft in height) of rectangular cross-section ( loses heat by radiation (transient) from all its surfaces to its surroundings at a temperature of eT . There is zero internal heat generation. = 2.00 ft by xL 2000 530 = = Determine the temperature of the billet (e.g. Node 625) after 3.7 hours ( × 1.3320 10 sec ). The bar is meshed with 432 elements: 12 elements along the height and 36 elements in the cross section. Analysis Summary: Dim. Type Load Material Geometry Contact Solver 3D Thermal Transient Thermal Linear Linear - Thermal Nonlinear Solution Method 3-Diagonal scaled conjugate gradient Units: lbf-s2/ft, ft, s, lbf, psf, lbf-ft (slug, foot, second, pound force, pound force/foot2, pound force-foot) - Thermal Energy is a Btu, Power is a Btu/s, 1 ∆ = ∆ 1F Dimensional Data: xL = 2.00 ft , yL = 2.00 ft , zL = 2.00 ft Material Data: Mass Density Heat Capacity × 4.875 10 = 1.100 10 × lbf − − / / Btu lbf − Btu ft / ft − (arbitrary value) ρ= pC = ε= Thermal Conductivity Emissivity × 1.000 10 1.000 Stefan-Boltzman = 4.750 10 × − 13 /Btu s − ft − Load: Thermal (billet) Thermal (outside) eT = = Element Types: 2000.0 530.0 (constant) (surroundings) Fully integrated S/R solid (elform=2) Material Models: Results Comparison: LS-DYNA temperature of the billet at selected point x=2.000 ft, y=2.010 ft, z= 0.000 ft (Node 625) is compared with R. Siegal and J.R. Howell studies in Thermal Radiation Heat Transfer, 1981, pg. 229. Reference Condition - Billet Temperature ( R ) at t=13320 sec Siegal and Howell [1981] Node 625 1.0000 10× 1.0080 10× The fully integrated selectively reduced solid element (elform=2) model provides a reasonable temperature comparison for this mesh (less that 1% difference). With the given simple geometry plus the initial temperature and radiation heat losses being space invariant, the temperature is uniform throughout the mesh. The temperature history of Node 625 used in the comparison is shown in Figure 25.2. *TITLE Cooling of a Billet Via Radiation *CONTROL_SOLUTION $# soln nlq isnan lcint 1 0 0 0 *CONTROL_THERMAL_SOLVER $# atype ptype solver cgtol gpt eqheat fwork sbc 1 2 3 1.00e-06 1 1.000000 1.0000004.7500e-13 *CONTROL_THERMAL_NONLINEAR $# refmax tol dcp 20 1.000e-06 0.500000 *CONTROL_THERMAL_TIMESTEP $# ts tip its tmin tmax dtemp tscp 1 0.500000 0.100000 0.100000 100.0000 1.000000 0.500000 *CONTROL_TERMINATION $# endtim endcyc dtmin endeng endmas 1.3320e+04 0 0.0 0.0 0.0 *DATABASE_TPRINT $# dt binary lcur ioopt 10.00000 0 0 1 *DATABASE_HISTORY_NODE $# nid1 nid2 nid3 nid4 nid5 nid6 nid7 nid8 1 13 79 265 *DATABASE_BINARY_D3PLOT $# dt lcdt beam npltc psetid 100.0000 0 0 0 0 *PART $# title Part 1 for TMat 1 and Elem Type 2 $# pid secid mid eosid hgid grav adpopt tmid 1 1 0 0 0 0 0 1 *SECTION_SOLID $# secid elform aet 1 2 1 *MAT_THERMAL_ISOTROPIC $# tmid tro tgrlc tgmult 1 487.5000 0.0 0.0 $# hc tc 0.11000 1.000e+04 *BOUNDARY_RADIATION_SET $# ssid type 1 1 $# flcid fmult tilcid timult loc 04.7500e-13 0 530.0000 0 *INITIAL_TEMPERATURE_SET $# nsid temp loc 1 2000.0000 0 *SET_NODE_LIST_TITLE all $# sid da1 da2 da3 da4 1 0.0 0.0 0.0 0.0 $# nid1 nid2 nid3 nid4 nid5 nid6 nid7 nid8 1 2 3 4 5 6 7 8 633 634 635 636 637 *SET_SEGMENT_TITLE rad_surf $# sid da1 da2 da3 da4 1 0.0 0.0 0.0 0.0 $# n1 n2 n3 n4 a1 a2 a3 a4 92 93 2 1 0.0 0.0 0.0 0.0 545 546 637 636 0.0 0.0 0.0 0.0 *ELEMENT_SOLID $# eid pid n1 n2 n3 n4 n5 n6 n7 n8 $# nid x y z tc rc 1 0.0 0.0 0.0 637 2.00000000 2.00000000 4.00000000 *END Notes: 1. The problem must be flagged as nonlinear if any boundary condition parameter is a function of temperature T. This includes a linear (i.e., straight line) relationship. 4T temperature Iterations are needed to obtain the correct solution. Radiation (q) is a boundary condition (usually F=1): = σε F T ( surface − ∞ ) 2. The *CONTROL_THERMAL_NONLINEAR keyword is optional. For example, the default values for remax (maximum number of iterations allowed per time step), tol (temperature convergence tolerance), and dcp (divergence control tolerance) will be used, if the nonlinear keyword is omitted, with ptype>0 on *CONTROL_ THERMAL_SOLUTION keyword. 3. This study could have been performed using a single element with the following modifications to the above input deck: *SET_NODE_LIST_TITLE all 1 0.0 0.0 0.0 0.0 1 2 3 4 5 6 7 8 *SET_SEGMENT_TITLE ext_surf $# sid da1 da2 da3 da4 1 0.0 0.0 0.0 0.0 $# n1 n2 n3 n4 a1 a2 a3 a4 2 3 7 6 0.0 0.0 0.0 0.0 7 8 5 6 0.0 0.0 0.0 0.0 4 8 7 3 0.0 0.0 0.0 0.0 2 6 5 1 0.0 0.0 0.0 0.0 4 1 5 8 0.0 0.0 0.0 0.0 1 4 3 2 0.0 0.0 0.0 0.0 *ELEMENT_SOLID $# eid pid n1 n2 n3 n4 n5 n6 n7 n8 1 1 1 2 3 4 5 6 7 8 *NODE 1 0.0 0.0 0.0 2 2.00000000 0.0 0.0 3 2.00000000 2.00000000 0.0 4 0.0 2.00000000 0.0 5 0.0 0.0 4.00000000 6 2.00000000 0.0 4.00000000 7 2.00000000 2.00000000 4.00000000 8 0.0 2.00000000 4.00000000 This single element representation provides the identical temperature result at t=3.7 hours ( ) as the 432 element mesh. × 1.3320 10 sec 26. Pipe Whip Keywords: *CONTROL_CONTACT *CONTACT_AUTOMATIC_SURFACE_TO_SURFACE_TITLE *MAT_PLASTIC_KINEMATIC *MAT_RIGID *INITIAL_VELOCITY_GENERATION *CONSTRAINED_EXTRA_NODES_SET Description: This problem illustrates the capabilities of LS-DYNA in a high speed, large deformation event with complex contact conditions, e.g. a pipe-on-pipe impact. The pipes are modeled using fully integrated shell elements. The impacted pipe is fully restrained, translationally and rotationally, at both ends ( and initial angular speed of 75 rad/s about a fixed point at one end (Figures 26.1 and 26.2). x = = ), while the impacting pipe is rotating at an x L= : = = = = = The pipe material is elastic-perfectly plastic, and the material model *MAT_PLASTIC_ KINEMATIC with zero tangent modulus is appropriate. The initial rotational velocity is imposed through the keyword *INITIAL_VELOCITY_ GENERATION. A rigid, rotational end joint is defined using the pipe's end ring of nodes which are made rigid using the *CONSTRAINED_EXTRA_NODES_SET and *MAT_RIGID keywords. The contact is *CONTACT_AUTOMATIC_SURFACE_TO_SURFACE. This contact has the following characteristics: • it is a two-way contact, in that user-specified slave nodes are checked for penetration of the master segments and then a second time, to check the master-side nodes for penetration through the slave segments, the treatment is thus symmetric and the definition of the slave surface and master surface is arbitrary, • • AUTOMATIC contacts check for penetration on either side of a shell element, • this is a recommended contact type in large deformation application, e.g. in crash simulations, since the orientation of parts relative to each other cannot always be anticipated. Shell thickness is considered with option shlthk=1. The soft=2 option (segment based Figure 26.1 – Finite element model with boundary condition nodes (marked with 's ). There are100 elements axially and 40 elements circumferentially. Figure 26.2 – Half-symmetry finite element model of a 50 in Analysis Summary: Dim. Type Load Material Geometry Contact Solver Solution Method 3D Dynamic Velocity Non- linear Linear 3D Explicit Units: lbf-s2/in, in, s, lbf, psi, lbf-in (blob, inch, second, pound force, pound force/inch2, pound force-inch) Dimensional Data: = = 5.000 10 × in , = 4.320 10 × in− Material Data: Mass Density Young's Modulus Poisson's Ratio Yield Stress Tangent Modulus Load: Velocity Element Types: = 7.324 10 × − lbf − / in lbf / in lbf / in × 3.000 10 0.3 4.500 10 × = ν = σ = tE = 0.000 10 × lbf / in ω= 7.500 10 × rad s / Fully integrated shell (elform=16) Material Models: *MAT_003 or *MAT_PLASTIC_KINEMATIC Results Comparison: The results for deformed shapes taken from R.M. Ferencz studies on Element-by-Element Preconditioning Techniques for Large-Scale, Vectorized Finite Element Analysis in Nonlinear Solid and Structural Mechanic, March, 1989 (pg. 142) are reproduced here in Figure 26.3. The LS-DYNA results for deformed shapes at selected times in the simulation (Figures 26.4a and 26.4b) are in good agreement. Figure 26.4a – Half-symmetry deformed shapes at 0.0025, 0.0050, 0.0100, and 0.0150 sec (hidden line view). Figure 26.4b – Half-symmetry deformed shapes at 0.0025, The histories of the kinetic energy, internal energy, sliding energy, and the total energy are given in Figure 26.5. Nearly all of the initial kinetic energy has been converted into plastic deformation (internal energy) due to the pipe deformation. There is a small amount of energy dissipated in the contact (sliding energy) between the pipes, which, when included in the output computation, makes for an energy balance. Figure 26.5 – Histories of the kinetic energy, internal energy, sliding energy, and the total energy. Input Deck: *KEYWORD *TITLE Pipe Whip *CONTROL_TERMINATION $# endtim endcyc dtmin endeng endmas 0.015000 0 0.0 0.0 0.0 *CONTROL_TIMESTEP $# dtinit tssfac isdo tslimt dt2ms lctm erode ms1st 0.0 0.900000 $# dt2msf dt2mslc imscl 0.0 0 0 *CONTROL_CONTACT $# slsfac rwpnal islchk shlthk penopt thkchg orien enmass 1.000000 0.0 2 2 0 0 1 0 0 0 0 4.000000 $# sfric dfric edc vfc th th_sf pen_sf 0.0 0.0 0.0 0.0 0.0 0.0 0.0 $# ignore frceng skiprwg 0 0 0 *CONTROL_ENERGY $# hgen rwen slnten rylen 2 2 2 2 *DATABASE_GLSTAT $# dt binary 1.0000e-05 1 *DATABASE_MATSUM $# dt binary 1.0000e-05 1 $# dt binary *DATABASE_SLEOUT 1.0000e-05 1 *DATABASE_BINARY_D3PLOT $# dt/cycl lcdt/nr beam npltc psetid 2.5000e-04 *PART $# title material type # 3 (Kinematic/Isotropic Elastic-Plastic) $# pid secid mid eosid hgid grav adpopt tmid 1 1 1 0 1 *SECTION_SHELL $# secid elform shrf nip propt qr/irid icomp setyp 1 16 0.83333 5.0 1 0.0 0 1 $# t1 t2 t3 t4 nloc marea 0.432000 0.432000 0.432000 0.432000 0 0.0 *MAT_PLASTIC_KINEMATIC $# mid ro e pr sigy etan beta 1 7.324e-04 3.000e+07 0.300000 4.500e+04 0.0 0.0 $# src srp fs vp 0.0 0.0 0.0 0.0 *HOURGLASS $# hgid ihq qm ibq q1 q2 qb qw 1 0 0.0 0 0.0 0.0 0.0 0.0 *PART $# title material type # 3 (Kinematic/Isotropic Elastic-Plastic) $# pid secid mid eosid hgid grav adpopt tmid 2 2 2 0 2 0 1 *SECTION_SHELL $# secid elform shrf nip propt qr/irid icomp setyp 2 16 0.83333 5.0 1 0.0 0 1 $# t1 t2 t3 t4 nloc marea 0.432000 0.432000 0.432000 0.432000 0 0.0 *MAT_PLASTIC_KINEMATIC $# mid ro e pr sigy etan beta 2 7.324e-04 3.000e+07 0.300000 4.500e+04 0.0 0.0 $# src srp fs vp 0.0 0.0 0.0 0.0 *HOURGLASS $# hgid ihq qm ibq q1 q2 qb qw 2 0 0.0 0 0.0 0.0 0.0 0.0 *PART $# title material type # 20 (Rigid) $# pid secid mid eosid hgid grav adpopt tmid 99 99 99 *SECTION_SHELL $# secid elform shrf nip propt qr/irid icomp setyp 99 2 0.83333 1.0 1 0.0 0 1 $# t1 t2 t3 t4 nloc marea 0.432000 0.432000 0.432000 0.432000 0 0.0 *MAT_RIGID $# mid ro e pr n couple m alias 99 7.324e-04 3.000e+07 0.300000 0.0 0.0 0.0 $# cmo con1 con2 $#lco or a1 a2 a3 v1 v2 v3 0.0 0.0 0.0 0.0 0.0 0.0 *CONSTRAINED_EXTRA_NODES_SET $# pid nsid 99 99 *SET_NODE_LIST_TITLE rigid ring of nodes $# sid da1 da2 da3 da4 solver 99 0.000 0.000 0.000 0.000MECH $# nid1 nid2 nid3 nid4 nid5 nid6 nid7 nid8 8041 8042 8043 8044 8045 8046 8047 8048 8049 8050 8051 8052 8053 8054 8055 8056 8057 8058 8059 8060 8061 8062 8063 8064 8065 8066 8067 8068 8069 8070 8071 8072 8073 8074 8075 8076 8077 8078 8079 8080 *INITIAL_VELOCITY_GENERATION $# id styp omega vx vy vz ivatn icid 2 2 75.000 0.0 0.0 0.0 0 0 $# xc yc zc nx ny nz phase irigid 25.000000 50.000000 6.725000 1.000000 0.0 0.0 0 0 *CONTACT_AUTOMATIC_SURFACE_TO_SURFACE_TITLE $# cid title 1 $# ssid msid sstyp mstyp sboxid mboxid spr mpr 1 2 3 3 0 0 0 0 $# fs fd dc vc vdc penchk bt dt 0.0 0.0 0.0 0.0 0.0 0 0.0 0.0 $# sfs sfm sst mst sfst sfmt fsf vsf 0.0 0.0 0.0 0.0 0.0 0.0 0.0 0.0 $# soft sofscl lcidab maxpar sbopt depth bsort frcfrq 2 0.100000 0 1.025 0.0 2 10 1 $# penmax thkopt shlthk snlog isym i2d3d sldthk sldstf 0.0 0 1 0 0 0 0.0 0.0 $# igap ignore 2 0 *ELEMENT_SHELL $# eid pid n1 n2 n3 n4 n5 n6 n7 n8 1 1 1 2 42 41 0 0 0 0 8000 2 8040 8001 8041 8080 0 0 0 0 *NODE $# nid x y z tc rc 1 0.000 28.096500 0.000 0 0 8080 28.058376 50.000000 7.209399 0 0 *SET_NODE_LIST $# sid da1 da2 da3 da4 solver 1 0.000 0.000 0.000 0.000MECH $# nid1 nid2 nid3 nid4 nid5 nid6 nid7 nid8 1 2 3 4 5 6 7 8 9 10 11 12 13 14 15 16 17 18 19 20 21 22 23 24 25 26 27 28 29 30 31 32 33 34 35 36 37 38 39 40 *SET_NODE_LIST $# sid da1 da2 da3 da4 solver 2 0.000 0.000 0.000 0.000MECH $# nid1 nid2 nid3 nid4 nid5 nid6 nid7 nid8 4001 4002 4003 4004 4005 4006 4007 4008 4009 4010 4011 4012 4013 4014 4015 4016 4017 4018 4019 4020 4021 4022 4023 4024 4025 4026 4027 4028 4029 4030 4031 4032 4033 4034 4035 4036 4037 4038 4039 4040 *BOUNDARY_SPC_SET $#nid/nsid cid dofx dofy dofz dofrx dofry dofrz 1 0 1 1 1 1 1 1 *BOUNDARY_SPC_SET $#nid/nsid cid dofx dofy dofz dofrx dofry dofrz 2 0 1 1 1 1 1 1 Notes: 1. The general contact *CONTACT_AUTOMATIC_SINGLE_SURFACE could also have been used. This type of contact has the following characteristics: • a single contact surface is created for all the parts included in the contact, • self contact is considered, • it is robust, reliable and accurate, making it the ideal choice for crashworthiness and impact applications. By default, if ssid (slave segment id) is zero or blank, all part IDs are included in the contact. A *PART_SET entry can be used to reduce the size of the part list. 2. The most common contact-related output file, rcforc, is produced by including a *DATABASE_RCFORC keyword in the input deck. rcforc is an ASCII file containing resultant contact forces for the slave and master sides of each contact interface. The forces are provided in the global coordinate system. Note that rcforc data is not provided for single surface contacts as all the contact forces from this contact type come from the slave side (as there is no master side) and thus the net contact forces are zero. To obtain rcforc data when single surface contacts are used, one or more force transducers should be added via the *CONTACT_FORCE_ TRANSDUCER_PENALTY keyword. A force transducer simply measures contact forces produced by other contact interfaces defined in the model. 3. By including a *DATABASE_SLEOUT keyword, individual contact interface energies are written to the ASCII output file sleout. The global contact energy is 27. Copper Bar Impacting a Rigid Wall Keywords: *CONTROL_ALE *CONTROL_CONTACT *CONTACT_AUTOMATIC_SURFACE_TO_SURFACE *RIGIDWALL_PLANAR *INITIAL_VELOCITY_GENERATION *SECTION_SOLID *HOURGLASS Description: This problem is known in the literature as "Taylor Bar Impact Test" and is used to assess material properties (plastic flow) under dynamic conditions. A deformable copper bar impacts a rigid wall at high speed. The deformed length (shortening), spread (widening), and maximum effective plastic strain (εp ) of the bar is determined. The contact of the deformable body and the rigid wall can be modeled in one of the following ways: • rigid wall (*RIGIDWALL_PLANAR), which provides an easy way to treat contact between a rigid-flat surface and the nodes of a deformable body, • using geometric entities (*CONTACT_ENTITY), • using a wall modeled with rigid shell elements and a *CONTACT_AUTOMATIC_ SURFACE_TO_SURFACE. Two of these methods are demonstrated for rigid wall contact, (1) the rigid wall is modeled with rigid shell elements (penalty method) and (2) the wall is modeled as a planar rigid boundary. The latter uses a constraint method which represents a perfectly plastic impact since, once penetration into the rigid wall is detected, the acceleration and velocity of the nodes are set to zero. No friction is included. The material is elastic-plastic with constant tangent stiffness and the material model *MAT_PLASTIC_KINEMATIC is used. For comparison, different solid hexahedron (elform=1,2,-2,-1) and tetrahedron (elform=10,13) elements, are used to model the bar as shown in Figure 27.1. Hourglass control is used with the default value (ihq=2 - Flanagan-Belytschko viscous form with coefficient qm=0.10) for the one-point quadrature element formulations. Traditional Lagrangian approaches, for large deformations, often result in highly distorted meshes for the elements close to the impacted region, leading to loss of accuracy and decreasing the critical time step for the simulation. Therefore, a simple Arbitrary Lagrangian-Eulerian (ALE) formulation (elform=5) is also presented. A mix of simple average smoothing and volume weighted smoothing is used for the interior nodal The (elform=5) formulation is single material ALE with Lagrange outer boundary node treatment and mesh smoothing effective for only moderate deformation. Thus application of this formulation is limited to mostly academic problems, since there are not many practical applications for use of this feature. In fact, this "Taylor Bar Impact Test" may be the only known practical application. Figure 27.1 – Finite element models of the impacting bar using hexahedron and tetrahedron elements (shell elements were used to model the impacted rigid plate). Each of these solid element meshes has 36 elements axially. There are 288 and 1440 elements per row for the hexahedron and tetrahedron models, respectively. Analysis Summary: Dim. Type Load Material Geometry Contact Solver 3D Dynamic Velocity Non- linear Non- linear 3D Explicit Solution Method Lagrangian and ALE Units: g, mm, ms, N, MPa, N-mm (gram, millimeter, millisecond, Newton, MegaPascal, Newton- Dimensional Data: = 3.240 10 × mm , = 6.400 10 × mm Material Data: Mass Density = − × × 8.930 10 1.170 10 0.35 4.000 10 × /g mm MPa MPa 1.000 10 × MPa = ν = σ = tE = zV = 2.270 10 × mm ms / Young's Modulus Poisson's Ratio Yield Stress Tangent Modulus Load: Velocity Element Types: Constant stress solid (elform=1) Fully integrated S/R solid (elform=2) Fully integrated S/R solid - for poor aspect ratio (acc) - (elform=-2) Fully integrated S/R solid - for poor aspect ratio (eff) - (elform=-1) 1 point tetrahedron (elform=10) 1 point nodal pressure tetrahedron (elform=13) 1 point ALE (elform=5) Material Models: *MAT_003 or *MAT_PLASTIC_KINEMATIC *MAT_020 or *MAT_RIGID Results Comparison: The results for deformed shapes at 0.0, 5, 20, and 80 ms, taken from R.M. Ferencz studies on Element-by-Element Preconditioning Techniques for Large-Scale, Vectorized Finite Element Analysis in Nonlinear Solid and Structural Mechanics, March, 1989 (pg. 86), are reproduced here in Figure 27.2. Ferencz [1989] used NIKE3D and its implicit dynamics solver. The LS-DYNA results for deformed shapes at 80.0 ms (Figures 27.3a to 27.3g) using penalty method contact and rigid boundary contact (Figures 27.7a to ) given 27.7g) are in good agreement. The maximum effective plastic strain ( by Ferencz [1989] differs significantly from the non-ALE results of LS-DYNA 2.248 2.9 ε ≅p ( from the highly distorted elements in the vicinity of the rigid wall. ), even though both use a Lagrangian approach; these values are taken 3.9 to Figure 27.2 – Deformed shapes (Ferencz [1989]) at 0.0, 5, 20, and 80 ms. Penalty Method (Rigid Mesh Material) Shortening (mm) Widening (mm) Max. plastic strain (εp ) Normalized CPU Time Constant stress solid (elform=1) Fully integrated S/R solid (elform=2) Fully integrated S/R solid (elform=-2) Fully integrated S/R solid (elform=-1) 1 point tetrahedron (elform=10) 1 point nodal pressure tetrahedron (elform=13) 1 point ALE (elform=5) 10.928 8.125 3.523 1.40 10.976 8.395 3.671 5.20 10.972 8.404 3.663 19.40 10.976 8.418 3.700 6.40 11.088 7.537 2.944 3.00 11.017 8.533 3.924 10.50 10.892 7.856 2.272 The above displacement and effective plastic strains results were obtained from the d3plot contour plots at 80.0 ms which were generated by the *DATABASE_BINARY_ D3PLOT keyword. Normalized CPU times shown in the above Penalty Method results table were normalized using the minimum value (the smallest value for all simulations - other contact type CPU times are to follow). Large effective plastic strains develop at the impact end of the rod due to the severe local mesh distortion, also resulting in reduced accuracy. For these simulations, a wide range of CPU times were associated with the different element formulations. The CPU time is controlled by the number of element operations required for that particular formulation, the complexity of the contact-impact approach and the element stable time step. The one-point quadrature (low order) constant stress solid (elform=1) element formulation (the LS-DYNA default), the higher order, fully integrated selectively reduced solid (elform=2), and the higher order, fully integrated S/R solid (both so-called efficient and accurate formulation choices) intended to address poor aspect ratios (elform=-1 and - 2, respectively), provide roughly the same dimensional changes and maximum effective plastic strain. The one-point quadrature (low order) tetrahedron (elform=10) element formulation provides comparatively stiffer dimensional changes and maximum effective plastic strain than the constant stress solid and fully integrated element formulations. This is probably due to this element formulation being prone to volumetric locking (overly stiff behavior) in incompressible regimes, e.g., as in plasticity. The one-point quadrature (low order) nodal pressure tetrahedron (elform=13) element formulation provides a less stiff, dimensional changes and maximum effective plastic strain comparison to that of the constant stress solid and fully integrated element formulations. This element formulation has no volumetric locking under plastic incompressible conditions. The one point ALE (elform=5) element formulation provides similar dimensional changes to other element formulations. With its nodal smoothing capability controlling the aspect ratio of the elements, mesh distortion is reduced, yet a smaller maximum effective plastic strain ( ) is achieved compared to the Lagrangian elements ε ≅p ( ). An explanation for these results is the moderate deformation to limitation for the one point ALE formulation. 2.272 ε =p 2.9 3.9 The LS-DYNA results for deformed shapes at 80.0 ms using penalty method contact with Figure 27.3a – Quarter-symmetry deformed shape (penalty method) with effective plastic strain contouring at 80 ms (elform=1). Figure 27.3b – Quarter-symmetry deformed shape (penalty method) Figure 27.3c – Quarter-symmetry deformed shape (penalty method) with effective plastic strain contouring at 80 ms (elform=-2). Figure 27.3d – Quarter-symmetry deformed shape (penalty method) Figure 27.3e – Quarter-symmetry deformed shape (penalty method) with effective plastic strain contouring at 80 ms (elform=10). Figure 27.3f – Quarter-symmetry deformed shape (penalty method) Figure 27.3g – Quarter-symmetry deformed shape (penalty method) with effective plastic strain contouring at 80 ms (elform=5). The half-symmetry deformed shape (penalty method contact), which illustrates the different element deformation for elform=1 and elform=5 at 80 ms, is given in Figure 27.4. Figure 27.4 – Half-symmetry deformed shape (penalty method) for elform=1 and elform=5 at 80 ms. The histories of the kinetic energy, internal energy, hourglass energy, sliding energy, and the total energy for (elform=1) of penalty method impact are given in Figure 27.5, while the histories of the stable time step increment for all elforms (1,2,-2,-1,10,13,5) Figure 27.5 – Histories of the kinetic energy, internal energy, hourglass energy, sliding energy, and the total energy for (elform=1) of penalty method impact. Figure 27.6 – Histories of the stable time step increment for all elforms Planar Rigid Boundary Shortening (mm) Widening (mm) Max. plastic strain (εp ) Normalized CPU Time Constant stress solid (elform=1) Fully integrated S/R solid (elform=2) Fully integrated S/R solid (elform=-2) Fully integrated S/R solid (elform=-1) 1 point tetrahedron (elform=10) 1 point nodal pressure tetrahedron (elform=13) 1 point ALE (elform=5) 10.897 7.889 3.243 1.00 10.936 8.139 3.366 3.40 10.933 8.182 3.394 14.00 10.936 8.183 3.405 4.10 11.044 7.201 3.057 2.70 10.987 8.214 4.288 9.00 10.886 7.716 2.272 3.60 The above displacement and effective plastic strains results were obtained from the d3plot contour plots at 80.0 ms which were generated by the *DATABASE_BINARY_ D3PLOT keyword. The more efficient rigid boundary contact procedure requires less CPU time (20% to 60%) than the penalty method for contact-impact. The exception is the one point ALE multi-material formulation, where the CPU times were about the same, probably due to the smoothing operations control. For all the element formulations (except the 1 point ALE) used, the contact-impact results provided using the penalty method and the planar rigid boundary differ due to the contact methods. Comments provided for the penalty method results regarding element formulation CPU times, the (elform=1,2,-2,-1) similarities for dimensional changes and maximum effective plastic strain, the (elform=10) stiffer comparison, the (elform=13) less stiff comparison, and the (elform=5) similarity and difference are also appropriate for the rigid boundary contact results. The LS-DYNA results for deformed shapes at 80.0 ms using rigid boundary contact with Figure 25.7a – Quarter-symmetry deformed shape (rigid boundary) with effective plastic strain contouring at 80 ms (elform=1). Figure 27.7b – Quarter-symmetry deformed shape (rigid boundary) Figure 27.7c – Quarter-symmetry deformed shape (rigid boundary) with effective plastic strain contouring at 80 ms (elform=-2). Figure 27.7d – Quarter-symmetry deformed shape (rigid boundary) Figure 27.7e – Quarter-symmetry deformed shape (rigid boundary) with effective plastic strain contouring at 80 ms (elform=10). Figure 27.7f – Quarter-symmetry deformed shape (rigid boundary) Figure 27.7g – Quarter-symmetry deformed shape (rigid boundary) with effective plastic strain contouring at 80 ms (elform=5). The half-symmetry deformed shape (planar rigid boundary contact), which illustrates the different element deformation for elform=1 and elform=5 at 80 ms, is given in Figure 27.8. Figure 27.8 – Half-symmetry deformed shape (rigid boundary) for elform=1 and elform=5 at 80 ms. The histories of the kinetic energy, internal energy, hourglass energy, sliding energy, and the total energy for (elform=1) of rigid boundary impact are given in Figure 27.9, while the histories of the stable time step increment for all elforms (1,2,-2,-1,10,13,5) Figure 27.9 – Histories of the kinetic energy, internal energy, hourglass energy, stonewall energy, and the total energy for (elform=1) of rigid boundary impact. Figure 27.10 – Histories of the stable time step increment for all elforms *TITLE Copper Bar Impacting a Rigidwall *CONTROL_TERMINATION $# endtim endcyc dtmin endeng endmas 8.000e-02 0 0.0 0.0 0.0 *CONTROL_TIMESTEP $# dtinit tssfac isdo tslimt dt2ms lctm erode ms1st 0.0 0.800000 0 0.0 0.0 $# dt2msf dt2mslc imscl 0.0 0 0 *CONTROL_CONTACT $# slsfac rwpnal islchk shlthk penopt thkchg orien enmass 0.100000 0.0 2 0 0 0 1 $# usrstr usrfrc nsbcs interm xpene ssthk ecdt tiedprj 0 0 0 0 4.00000 $# sfric dfric edc vfc th th_sf pen_sf 0.0 0.0 0.0 0.0 0.0 0.0 0.0 $# ignore frceng skiprwg 0 0 0 *CONTROL_ENERGY $# hgen rwen slnten rylen 2 2 2 2 *DATABASE_GLSTAT $# dt binary 5.0000e-04 1 *DATABASE_MATSUM $# dt binary 5.0000e-04 1 *DATABASE_SLEOUT $# dt binary 5.0000e-04 1 *DATABASE_RWFORC $# dt binary 5.0000e-04 1 *DATABASE_BINARY_D3PLOT $# dt/cycl lcdt/nr beam npltc psetid 1.0000e-03 *PART $# title material type # 3 (Kinematic/Isotropic Elastic-Plastic) $# pid secid mid eosid hgid grav adpopt tmid 1 1 1 0 1 *SECTION_SOLID $# secid elform aet 1 1 *MAT_PLASTIC_KINEMATIC $# mid ro e pr sigy etan beta 1 8.930e-03 1.170e+05 0.35000 4.000e+02 1.000e+02 0.0 $# src srp fs vp 0.0 0.0 0.0 0.0 *HOURGLASS $# hgid ihq qm ibq q1 q2 qb qw 1 0 0.0 0 0.0 0.0 0.0 0.0 *PART $# title material type # 20 (Rigid) $# pid secid mid eosid hgid grav adpopt tmid 2 2 2 0 2 *SECTION_SHELL $# secid elform shrf nip propt qr/irid icomp setyp 2 2 0.0 0 0 0.0 $# t1 t2 t3 t4 nloc marea 0.100000 0.100000 0.100000 0.100000 0 0.0 *MAT_RIGID $# mid ro e pr n couple m 2 8.930e-03 1.170e+05 0.35000 0.0 0.0 0.0 1.000000 7 7 $#lco or a1 a2 a3 v1 v2 v3 0.0 0.0 0.0 0.0 0.0 0.0 *HOURGLASS $# hgid ihq qm ibq q1 q2 qb qw 2 0 0.0 0 0.0 0.0 0.0 0.0 *CONTACT_AUTOMATIC_SURFACE_TO_SURFACE_TITLE $# cid title 1copper bar-rigidwall interface $# ssid msid sstyp mstyp sboxid mboxid spr mpr 1 2 3 3 $# fs fd dc vc vdc penchk bt dt 0.0 0.0 0.0 0.0 0.0 0 0.0 0.0 $# sfs sfm sst mst sfst sfmt fsf vsf 0.0 0.0 0.0 0.0 0.0 0.0 0.0 0.0 $# soft sofscl lcidab maxpar sbopt depth bsort frcfrq 2 0.100000 0 1.025 0.0 2 10 1 $# penmax thkopt shlthk snlog isym i2d3d sldthk sldstf 0.0 0 1 0 0 0 0.0 0.0 $# igap ignore 2 0 *INITIAL_VELOCITY_GENERATION $# id styp omega vx vy vz ivatn icid 1 2 0.0 0.0 0.0 -227.00 0 0 $# xc yc zc nx ny nz phase irigid 0.0 0.0 0.0 0.0 0.0 0.0 0 0 *ELEMENT_SOLID $# eid pid n1 n2 n3 n4 n5 n6 n7 n8 1 1 1 10 11 2 306 315 316 307 10368 1 10900 10683 10684 10748 11205 10988 10989 11053 *ELEMENT_SHELL $# eid pid n1 n2 n3 n4 n5 n6 n7 n8 10369 2 11299 11300 11287 11286 0 0 0 0 10512 2 11453 11454 11441 11440 0 0 0 0 *NODE $# nid x y z tc rc 1 1.131371 1.131371 0.000 0 0 11285 -0.848528 -0.848528 32.400000 0 0 11286 10.000000 -10.000000 -0.100000 0 0 11454 -10.000000 10.000000 -0.100000 0 0 *END Notes: 1. If a part is comprised entirely of tetrahedrons, there are several tetrahedral formulations to choose from, each with various pros and cons. Any of these formulations are preferable to using degenerate, elform=1 tetrahedrons. Two popular choices are (a) elform=10 which is 1 point tetrahedron with 4 nodes, but prone to volumetric locking (overly stiff behavior) in incompressible regimes, e.g., as in metal plasticity, and (b) elform=13 which is a 1 point nodal pressure tetrahedron developed for bulk metal forming; elform=13 is identical with elform=10 with addition of nodal pressure averaging that significantly decreases volumetric locking. There are also two relatively new 10-noded tetrahedron, elform=16 and 17 which have not been widely used. 2. To convert from a Lagrangian simulation to an ALE, the user needs to add the logic (dct), cycle between advection (nadv), advection method (meth), smoothing weight factors (afac thru efac), etc.: *CONTROL_ALE $# dct nadv meth afac bfac cfac dfac efac -1 1 2 0.500000 0.500000 0.0 0.0 0.0 $# start end aafac vfact vlimit ebc pref 0.0 1.000e+20 1.000000 1.000e-06 0.0 0 0.0 and modify the element formulation choice: *SECTION_SOLID $# secid elform aet 1 5 3. Hexahedral elements with reasonable aspect ratios should be used for the initial ALE mesh. Degenerate element shapes, such as tetrahedrons and pentahedrons, should be avoided as they lead to reduced accuracy and perhaps numerical instability during the advection. 4. The viscous contact damping parameter, vdc, on card 2 of the *CONTACT_ AUTOMATIC_SURFACE_TO_SURFACE keyword is zero by default. Contact damping is often beneficial in reducing high-frequency oscillation of contact forces in crash or impact simulations. In contacts involving soft materials such as foams and honeycombs, instabilities exist due to contact oscillations. Using a value of vdc between 40-60 (corresponding to 40% to 60% of critical damping), improves stability; however, it may be necessary to reduce the time step scale factor. Generally, a smaller value of vdc, say equal to 20, is recommended when metals, which have similar material stiffnesses, interact. 5. Contact-impact results using penalty method and planar rigid boundaries can possible differ due to their approaches. The penalty method consists of placing normal interface springs between all penetrating nodes and the contact surface. The rigid boundary contact procedure for stopping nodes uses a constraint method which represents a perfectly plastic impact that results in an irreversible energy loss. The total energy dissipated is found by taking the difference between the total kinetic energy of all the nodal points slaved to the rigid wall before and after the impact with the wall. The advantage of the constraint method is that it guarantees the node to lie on the positive side of the rigidwall (no penetration). 6. To move from the contact-impact model used by the penalty method, i.e. that with a meshed rigid wall, to a planar rigid boundary model, the user needs to remove the following entries used to represent the contact-impact and the meshed rigid wall: *CONTROL_CONTACT $# slsfac rwpnal islchk shlthk penopt thkchg orien enmass 0.100000 0.0 2 0 0 0 1 $# usrstr usrfrc nsbcs interm xpene ssthk ecdt tiedprj 0 0 0 0 4.00000 $# sfric dfric edc vfc th th_sf pen_sf 0.0 0.0 0.0 0.0 0.0 0.0 0.0 $# title material type # 20 (Rigid) $# pid secid mid eosid hgid grav adpopt tmid 2 2 2 0 2 *SECTION_SHELL $# secid elform shrf nip propt qr/irid icomp setyp 2 2 0.0 0 0 0.0 $# t1 t2 t3 t4 nloc marea 0.100000 0.100000 0.100000 0.100000 0 0.0 *MAT_RIGID $# mid ro e pr n couple m 2 8.930e-03 1.170e+05 0.35000 0.0 0.0 0.0 $# cmo con1 con2 1.000000 7 7 $#lco or a1 a2 a3 v1 v2 v3 0.0 0.0 0.0 0.0 0.0 0.0 *HOURGLASS $# hgid ihq qm ibq q1 q2 qb qw 2 0 0.0 0 0.0 0.0 0.0 0.0 *CONTACT_AUTOMATIC_SURFACE_TO_SURFACE_TITLE $# cid title 1copper bar-rigidwall interface $# ssid msid sstyp mstyp sboxid mboxid spr mpr 1 2 3 3 $# fs fd dc vc vdc penchk bt dt 0.0 0.0 0.0 0.0 20.0 0 0.0 0.0 $# sfs sfm sst mst sfst sfmt fsf vsf 0.0 0.0 0.0 0.0 0.0 0.0 0.0 0.0 $# soft sofscl lcidab maxpar sbopt depth bsort frcfrq 2 0.100000 0 1.025 0.0 2 10 1 $# penmax thkopt shlthk snlog isym i2d3d sldthk sldstf 0.0 0 1 0 0 0 0.0 0.0 $# igap ignore 2 0 *ELEMENT_SHELL $# eid pid n1 n2 n3 n4 n5 n6 n7 n8 10369 2 11299 11300 11287 11286 0 0 0 0 10512 2 11453 11454 11441 11440 0 0 0 0 *NODE $# nid x y z tc rc 11286 10.000000 -10.000000 -0.100000 0 0 11454 -10.000000 10.000000 -0.100000 0 0 and replace them with the following planar rigid boundary entry (the user can also include the rigid wall force entry if desired): *DATABASE_RWFORC $# dt binary 5.0000e-04 1 *RIGIDWALL_PLANAR $# nsid nsidex boxid offset birth death rwksf 0 0 0 $# xt yt zt xh yh zh fric wvel Implicit Studies: NIKE3D (implicit dynamics solver) was used by Ferencz [1989] with the computation divided into 80 time steps of 1 microsecond and nodal boundary conditions constraining the impacting face to lie on the global X-Y plane. The half-symmetry deformed shape, at 80 ms (final state), is shown in Figure 27.11. NIKE3D uses an element formulation, similar to the selected reduced integration of LS- DYNA (elform=2), defined as B-Bar method. The selective reduced integration splits the stress tensor into deviatoric and dilatation (mean) parts, whereas the B-Bar method splits the B matrix (a strain modification) into dilatational and deviatoric parts. The contact of the deformable body and the rigid wall can be modeled in one of the following ways in this study: • using nodal boundary conditions which constrain the impacting face to remain on the • rigid wall, rigid wall (*RIGIDWALL_PLANAR), which provides an easy way to treat contact between a rigid-flat surface and the nodes of a deformable body. In general, there are two different methods that are available in LS-DYNA to treat nodes impacting a rigid wall. The first method, which is the default method, is the constraint type that is used for all deformable nodes impacting a rigid wall. The second (optional) method is the penalty approach that is used for all rigid nodes or optional deformable nodes impacting the rigid wall. The primary difference between the two methods is in the conservation of energy and momentum. If using the implicit solver, only the penalty approach method is available. The default constraint method does not conserve momentum and the energy. This is due to the fact that when a deformable node is found to penetrate a rigidwall, its velocity is immediately reset to zero and is moved back onto the surface of the rigidwall. The advantage of the constraint method is that it always guarantees the node to lie on the positive side of the rigidwall (no penetration). The penalty method (optional for explicit solver/default for implicit solver) for rigid walls uses a scale factor that can be adjusted (default is 1.0) by modifying the rwskf parameter on *RIGIDWALL_PLANAR keyword. This works the same as the contact-impact interface treatment. When a deformable or a rigid node is found to penetrate a rigidwall, the penetrated distance normal to the rigid wall is computed and is resisted by applying a force that is proportional to the computed distance multiplied by a stiffness factor that is based on the material of the impacting node and the dimensions of the attached element. Figure 27.11 – Half-symmetry deformed shape (Ferencz [1989]) at 80 ms (final state). Analysis Summary: Dim. Type Load Material Geometry Contact Solver 3D Dynamic Velocity Non- linear Non- linear SPC's Implicit and Dim. Type Load Material Geometry Contact Solver Solution Method 2-Nonlinear w/BFGS Solution Method 3D Dynamic Velocity Non- linear Non- linear R.Wall (penalty) Explicit/ Implicit 2-Nonlinear w/BFGS Element Type: Different Considerations from Explicit Solver: The contact of the deformable body and the rigid wall can be modeled in one of the following ways in this study: • using nodal boundary conditions which constrain the impacting face to remain on the • rigid wall, rigid wall (*RIGIDWALL_PLANAR), which provides an easy way to treat contact between a rigid-flat surface and the nodes of a deformable body. Studies 1 and 2: • NIKE3D and LS-DYNA (each using implicit dynamics solver) Comparison, and • Implicit LS-DYNA Convergence, with nodal boundary conditions constraining the impacting face for both studies. Nodal Boundary (SPC's) Shortening (mm) Widening (mm) Max. plastic strain (εp ) Normalized CPU Time B-Bar solid (NIKE3D) - 80 time steps Fully integrated S/R solid 80 time steps Fully integrated S/R solid 160 time steps Fully integrated S/R solid 320 time steps Fully integrated S/R solid 400 time steps Fully integrated S/R solid 480 time steps Fully integrated S/R solid 640 time steps Fully integrated S/R solid 800 time steps 11.446 7.68 est. 2.248 - 11.313 6.111 2.432 3.35 11.150 7.468 3.126 6.54 11.029 7.730 3.080 13.10 11.005 7.765 3.084 16.84 10.989 7.784 3.084 19.50 10.974 7.798 3.090 25.90 10.967 7.805 3.092 The above displacement and effective plastic strain results were obtained from the d3plot contour plots at 80.0 ms which were generated by the *DATABASE_BINARY_ D3PLOT keyword. Normalized CPU times shown in the above Nodal Boundary Condition (SPC's) results table were normalized using the explicit fully integrated S/R solid (elform=2) value. In the implicit solver direct comparison (80 time steps) of NIKE3D which uses the B-Bar element formulation and the selected reduced integration element formulation of LS- DYNA (elform=2), similar maximum effective plastic strain results ( vs. ε =p ) and length shortening (11.446 mm vs. 11.313 mm) are obtained. For some unexplained reason, the widening profiles (7.680 mm vs. 6.111 mm) differ significantly. 2.248 2.432 ε =p 2.432 ) is significantly less than the explicit solver value ( The maximum effective plastic strain obtained using the LS-DYNA implicit solver ε =p ( - initial work with penalty contact condition). This is believed to be due to the relatively large time step increment used (only 80 steps) which fails to capture the correct dynamics of the simulation. It is shown in above table that increasing the number of time steps (reducing the time step increment) allows the implicit solver to more accurately capture the rate of material deformation (plastic flow) and appears to be converging to a unique solution ε =p ( and 7.810 mm) with a consistent shape profile. 3.366 3.100 ε =p The half-symmetry deformed shape (nodal boundary constraint) with widening profiles and effective plastic strain contouring for selected implicit integration time step sizes at 80 ms, are given in Figures 27.12 (80 time steps), 27.13 (160 time steps), and 27.14 (640 time steps). Figure 27.12 provides a LS-DYNA deformed shape (80 time steps) comparison with the NIKE3D result (80 time steps) shown in Figure 27.11. Together, and 7.468 mm), and 27.14 Figures 27.12 ( ε =p ( and 7.798 mm) illustrate the LS-DYNA converging results with increasing the number of time steps (reducing the time step increment). and 6.111 mm), 27.13 ( 3.090 3.126 2.432 ε =p ε =p Unfortunately, as is shown in above table, the CPU time becomes a deterrent when using implicit dynamics solvers. Thus, the explicit solver is often favored for these types of high deformation, impact simulations due to its ability to provide efficient and stable Figure 27.12 – Half-symmetry widening and effective plastic strain contouring with nodal boundary conditions - 80 time steps. Figure 27.13 – Half-symmetry widening and effective plastic strain contouring with Figure 27.14 – Half-symmetry widening and effective plastic strain contouring with nodal boundary conditions - 640 time steps. Input deck: *KEYWORD *TITLE Copper Bar Impacting a Rigidwall *CONTROL_IMPLICIT_DYNAMICS $# imass gamma beta 1 0.500000 0.250000 *CONTROL_IMPLICIT_GENERAL $# imflag dt0 imform nsbs igs cnstn form 1 0.00100 0 0 0 $ 1 0.00050 0 0 0 $ 1 0.00025 0 0 0 $ 1 0.00020 0 0 0 $ 1 0.0001666 0 0 0 $ 1 0.0001250 0 0 0 $ 1 0.00010 0 0 0 *CONTROL_IMPLICIT_SOLVER $# lsolvr prntflg negeig order drcm drcprm autospc aspctl 4 2 2 0 1 0 1 0 $# lcpack 2 *CONTROL_IMPLICIT_SOLUTION $# nsolvr ilimit maxref dctol ectol rctol stol abstol 2 11 15 0.0010 0.0100 1.00e+10 0.900000 1.00e-10 $# dnorm diverg istif nlprint nlnorm d3itctl cpchk 2 1 1 2 $# arcctl arcdir arclen rcmth arcdmp 0 1 0.0 1 2 *CONTROL_TERMINATION $# endtim endcyc dtmin endeng endmas 3 0 3 0.0 0.0 0.0 *END Notes: Studies 3 and 4: • LS-DYNA Explicit Solver (with rigid wall constraint method contact) and Implicit Dynamics Solver (with rigid wall penalty method contact) Comparison, and • Implicit LS-DYNA Convergence. Planar Rigid Boundary Shortening (mm) Widening (mm) Max. plastic strain (εp ) Normalized CPU Time Fully integrated S/R solid Explicit - 9883 time steps Fully integrated S/R solid Implicit - 80 time steps Fully integrated S/R solid Implicit - 160 time steps Fully integrated S/R solid Implicit - 320 time steps Fully integrated S/R solid Implicit - 400 time steps Fully integrated S/R solid Implicit - 480 time steps Fully integrated S/R solid Implicit - 640 time steps Fully integrated S/R solid Implicit - 800 time steps Fully integrated S/R solid Implicit - 1600 time steps Fully integrated S/R solid Implicit - 3200 time steps 10.936 8.139 3.366 1.00 11.155 7.083 2.821 3.35 11.285 7.326 3.109 6.54 11.216 7.502 3.235 13.10 11.179 7.534 3.270 16.84 11.166 7.550 3.274 19.50 11.045 8.503 3.586 25.90 11.033 8.517 3.644 33.38 11.023 8.542 3.680 67.30 11.022 8.545 3.696 The above displacement and effective plastic strain results were obtained from the d3plot contour plots at 80.0 ms which were generated by the *DATABASE_BINARY_ D3PLOT keyword. Normalized CPU times shown in the above Rigid Wall Planar results table were normalized using the explicit fully integrated S/R solid (elform=2) value. ε =p 2.821 As for the previous nodal boundary condition method, the maximum effective plastic strain ( ) and widening profile (7.083 mm) for the 80 time step solution are ε =p roughly 15% less than the explicit results ( and 8.139 mm). As before, this is believed to be due to the relatively large time step increment used (only 80 steps) which fails to capture the correct dynamics of the simulation. It is shown that increasing the number of time steps (reducing the time step increment) allows the solver to better capture the rate of material deformation (plastic flow) which appears to be converging ε =p ( and 7.550 mm) over a range of time steps studied. 3.366 3.274 For some unexplained reason, starting with the 640 time step solution, there is a further increase in maximum effective plastic strain and widening results and a distinct change in the widening profile with the outer row of nodes now turning more upward. The ε =p and 8.545 mm) appear to be converging, though corresponding results ( greater than those provided by the explicit solver ( and 8.139 mm) which also has the outer row of nodes turning slightly upward. 3.366 3.696 ε =p The half-symmetry deformed shape (planar rigid boundary) with widening profiles and effective plastic strain contouring for selected implicit integration time step sizes at 80 ms, are given in Figures 27.15 (explicit), 27.16 (80 time steps), 27.17 (160 time steps), and 27.18 (640 time steps). Figure 27.15 provides a LS-DYNA widening and effective and 8.139 mm) for the explicit solver. Together, plastic strain results ( Figures 27.16 ( and 7.326 mm), and 27.18 ε =p ( and 8.503 mm) illustrate the LS-DYNA converging results for the implicit solver with increasing the number of time steps (reducing the time step increment). and 7.083 mm), 27.17 ( 3.366 2.821 3.109 3.586 ε =p ε =p ε =p Unfortunately, as is shown in above table, the CPU time becomes a deterrent when using implicit dynamics solvers. Thus, the explicit solver is often favored for these types of high deformation, impact simulations due to its ability to provide efficient and stable Figure 27.15 – Half-symmetry widening and effective plastic strain contouring with rigid boundary condition - explicit. Figure 27.16 – Half-symmetry widening and effective plastic strain contouring with Figure 27.17 – Half-symmetry widening and effective plastic strain contouring with rigid boundary condition - 160 time steps. Figure 27.18 – Half-symmetry widening and effective plastic strain contouring with *TITLE Copper Bar Impacting a Rigidwall *CONTROL_IMPLICIT_DYNAMICS $# imass gamma beta 1 0.500000 0.250000 *CONTROL_IMPLICIT_GENERAL $# imflag dt0 imform nsbs igs cnstn form 1 0.00100 0 0 0 $ 1 0.00050 0 0 0 $ 1 0.00025 0 0 0 $ 1 0.00020 0 0 0 $ 1 0.0001666 0 0 0 $ 1 0.0001250 0 0 0 $ 1 0.00010 0 0 0 $ 1 0.00005 0 0 0 $ 1 0.000025 0 0 0 *CONTROL_IMPLICIT_SOLVER $# lsolvr prntflg negeig order drcm drcprm autospc aspctl 4 2 2 0 1 0 1 0 $# lcpack 2 *CONTROL_IMPLICIT_SOLUTION $# nsolvr ilimit maxref dctol ectol rctol stol abstol 2 11 15 0.0010 0.0100 1.00e+10 0.900000 1.00e-10 $# dnorm diverg istif nlprint nlnorm d3itctl cpchk 2 1 1 2 $# arcctl arcdir arclen rcmth arcdmp 0 1 0.0 1 2 *CONTROL_TERMINATION $# endtim endcyc dtmin endeng endmas 8.000e-02 0 0.0 0.0 0.0 *RIGIDWALL_PLANAR $# nsid nsidex boxid offset birth death rwksf 0 0 0 5.0 *END Table of Contents page 1. Introduction............................................................................................................................... 1-1 2. Units........................................................................................................................................... 2-1 3. Getting Started........................................................................................................................... 3-1 3.1 3.2 3.3 Problem Definition........................................................................................................... 3-1 Input File Preparation..................................................................................................... 3-1 LS-DYNA solution ........................................................................................................... 3-4 4. The Next Step ............................................................................................................................ 4-1 4.1 4.2 Explicit Analysis (problem ex01.k)................................................................................. 4-1 Implicit Analysis (problem im01.k)................................................................................ 4-3 4.3 Heat Transfer Analysis (problem th01.k)...................................................................... 4-5 List of Examples Example 4-1 Aluminum cube deformation, explicit method (file: ex01.k) Example 4-2 Aluminum cube deformation, implicit method (file: im01.k) Example 4-3 Aluminum cube transient heat transfer analysis (file: th01.k) Example 4-4 Aluminum cube coupled thermal-stress solution (file: cp01.k) page 4-2 4-3 LS-DYNA Introduction 1. Introduction LS-DYNA is used to solve multi-physics problems including solid mechanics, heat transfer, and fluid dynamics either as separate phenomena or as coupled physics, e.g., thermal stress or fluid structure interaction. This manual presents “very simple” examples to be used as templates (or recipes). This manual should be used side-by-side with the “LS-DYNA Keyword User’s Manual”. The keyword input provides a flexible and logically organized database. Similar functions are grouped together under the same keyword. For example, under the keyword, *ELEMENT, are included solid, beam, and shell elements. The keywords can be entered in an arbitrary order in the input file. However, for clarity in this manual, we will conform to the following general block structure and enter the appropriate keywords in each block. 1. define solution control and output parameters 2. define model geometry and material parameters LS-DYNA Units 2. Units LS-DYNA requires a consistent set of units to be used. All parameters in this manual are in SI units. length General • • mass temperature • time • • pressure Mechanical units • density • Modulus of elasticity • yield stress • coefficient of expansion Thermal units • heat capacity • • heat generation rate thermal conductivity [m] [kg] [K] [sec] [Pa] [kg/m3] [Pa] [Pa] [m/m K] [J/kg K] [W/m K] LS-DYNA Getting Started 3. Getting Started 3.1 Problem Definition Consider the deformation of an aluminum block sitting on the floor with a pressure applied to the top surface. P = 70.e+05 Pa Aluminum 1100-O density modulus of elasticity Poisson Ratio coefficient of expansion heat capacity thermal conductivity 2700 kg/m3 70.e+09 Pa 0.3 23.6e-06 m/m K 900 J/kg K 220 W/m K 1m 3.2 Input File Preparation The first step is to create a mesh and define node points. Since we are just getting started, we will define the mesh as consisting of only 1 element and 8 node points as shown in the following figure. Also, we will use default values for many of the parameters in the input file, and therefore not have to enter them. 5 1 6 2 8 4 7 3 The “LS-DYNA Keyword User’s Manual” should be read side-by-side with this manual. The following steps are required to create the finite element model input file. *KEYWORD The first line of the input file must begin with *KEYWORD. This identifies the file as containing the “keyword” format instead of the “structured” format which can also be used . The first input block is used to define solution control and output parameters. As a minimum, the LS-DYNA Getting Started will apply the pressure load as a ramp from 0 Pa to 70.e+05 Pa during a time interval of 1 second. Therefore, the termination time is 1 second. Additionally, one of the many output options should be used to control the printing interval of results (e.g., *DATABASE_BINARY_D3PLOT). We will print the results every 0.1 seconds. *CONTROL_TERMINATION 1. *DATABASE_BINARY_D3PLOT .1 The second input block is used to define the model geometry, mesh, and material parameters. The following description and map may help to understand the data structure in this block. We have 1 part, the aluminum block, and use the *PART keyword to begin the definition of the finite element model. The keyword *PART contains data that points to other attributes of this part, e.g., material properties. Keywords for these other attributes, in turn, point elsewhere to additional attribute definitions. The organization of the keyword input looks like this. *PART pid sid mid *SECTION_SOLID sid *MAT_ELASTIC mid ρ E µ *ELEMENT_SOLID eid pid nid *NODE nid x y z The LS-DYNA Keyword User Manual should be consulted at this time for a description of the keywords used above. A brief description follows: *PART We have 1 part identified by part identification (pid=1). This part has attributes identified by section identification (sid=1) and material identification (mid=1). *SECTION_SOLID Parts identified by (sid=1) are defined as constant stress 8 node brick elements by this keyword. *MAT_ELASTIC Parts identified by (mid=1) are defined as an elastic material with a density LS-DYNA Getting Started *ELEMENT_SOLID Eight node solid brick elements identified by element identification (eid=1) have the attributes of (pid=1) and are defined by the node list (nid) *NODE The node identified by (nid) has coordinates x,y,z. Our finite element model consists of 1 element, 8 nodes, and 1 material. Keeping the above in mind, the data entry for this block looks like this. *PART aluminum block 1 1 1 *SECTION_SOLID 1 *MAT_ELASTIC 1 2700. 70.e+09 .3 *ELEMENT_SOLID 1 1 1 2 3 4 5 6 7 8 *NODE 1 0. 0. 0. 7 7 2 1. 0. 0. 5 0 3 1. 1. 0. 3 0 4 0. 1. 0. 6 0 5 0. 0. 1. 4 0 6 1. 0. 1. 2 0 7 1. 1. 1. 0 0 8 0. 1. 1. 1 0 The third input block is used to define boundary conditions and time dependent load curves. We are applying a load of 70.e+05 Pa to the top surface of the block defined by nodes 5-6-7-8. We will ramp the load up from 0 Pa to 70.e+05 Pa during a time interval of 1 second. Note that the first data entry in *LOAD_SEGMENT is a load curve identification number (lcid=1) which points to the load curve defined by the keyword *DEFINE_CURVE having that same (lcid) identification number. *LOAD_SEGMENT 1 1. 0. 5 6 7 8 *DEFINE_CURVE *END 1 0. 0. 1. 70.e+05 The last line in the input file must have the keyword *END. *END LS-DYNA Getting Started 3.3 LS-DYNA solution The vertical and horizontal displacement of node 7, calculated by LS-DYNA, are shown in the following 2 graphs. The solution to this simple problem can be calculated analytically. The LS- DYNA solution compares exactly with the analytical solution. The vertical displacement due to a 70.0e+05 Pa pressure load can be calculated by =∆ Pl = ( )( ) 70 105 + ( ) 70 09 + = 1.0e-04 m The horizontal displacement is lh µ =∆=∆ ( )( .03.0 0001 ) = LS-DYNA The Next Step 4. The Next Step This chapter builds on the simple example presented in the previous chapter. First, more detail is given about solving this problem using explicit analysis in section 4.1. Explicit analysis is well suited to dynamic simulations such as impact and crash analysis, but it can become prohibitively expensive to conduct long duration or static analyses. Static problems, such as sheet metal spring back after forming, are one application area for implicit analysis. Implicit analysis is presented in section 4.2. The difference between explicit and implicit is described. The problem is then presented as a heat transfer problem in section 4.3 and finally as a coupled thermal-stress problem in section 4.4. 4.1 Explicit Analysis (problem ex01.k) Explicit refers to the numerical method used to represent and solve the time derivatives in the momentum and energy equations. The following figure presents a graphical description of time t+∆t . . . . . . time t n1 n2 n3 explicit time integration. The displacement of node n2 at time level t+∆t is equal to known values of the displacement at nodes n1, n2, and n3 at time level t. A system of explicit algebraic equations are written for all the nodes in the mesh at time level t+∆t. Each equation is solved in-turn for the unknown node point displacements. Explicit methods are computational fast but are conditionally stable. The time step, ∆t, must be less than a critical value or computational errors will grow resulting in a bad solution. The time step must be less than the length of time it takes a signal traveling at the speed of sound in the material to traverse the distance between the node points. The critical time step for this problem can be calculated by ∆t ≤ ∆x = = ∆x 1. 70. ∗10 2700. = 1.96 ∗10 −4 sec To be safe, the default value used by LS-DYNA is 90% of this value or 1.77e-04 sec. Therefore, this problem requires 5,658 explicit time steps as compared with 10 implicit time steps . Note that the time step and scale factor can be set using the keyword *CONTROL_TIMESTEP. The input file for the 1-element aluminum cube example problem, presented in Chapter 3, is LS-DYNA The Next Step Example 4-1 Aluminum cube deformation, explicit method (file: ex01.k) PID MID SECID *KEYWORD *TITLE ex01.k – explicit analysis, problem 1 $ $--------------- define solution control and output parameters ---------------- $ *CONTROL_TERMINATION 1. *DATABASE_BINARY_D3PLOT .1 $ $--------------- define model geometry and material parameters ---------------- $ *PART aluminum block 1 1 1 *SECTION_SOLID 1 *MAT_ELASTIC 1 2700. 70.e+09 .3 *NODE 1 0. 0. 0. 7 7 2 1. 0. 0. 5 0 3 1. 1. 0. 3 0 4 0. 1. 0. 6 0 5 0. 0. 1. 4 0 NID 6 1. 0. 1. 2 0 7 1. 1. 1. 0 0 8 0. 1. 1. 1 0 *ELEMENT_SOLID 1 1 1 2 3 4 5 6 7 8 $ $---------------- define boundary conditions and load curves ------------------ $ *LOAD_SEGMENT 1 1. 0. 5 6 7 8 *DEFINE_CURVE 1 0. 0. 1. 70.e+05 *END LCID LS-DYNA The Next Step 4.2 Implicit Analysis (problem im01.k) Implicit refers to the numerical method used to represent and solve the time derivatives in the momentum and energy equations. The following figure presents a graphical description of time t+∆t . . . . . . time t n1 n2 n3 implicit time integration. The displacement of node n2 at time level t+∆t is equal to known values of the displacement at nodes n1, n2, and n3 at time level t, and also the unknown displacements of nodes n1 and n3 at time level t+∆t. This results in a system of simultaneous algebraic equations that are solved using matrix algebra (e.g., matrix inversion). The advantage of this approach is that it is unconditionally stable (i.e., there is no critical time step size). The disadvantage is the large numerically effort required to form, store, and invert the system of equations. Implicit simulations typically involve a relatively small number of computationally expensive time steps. The keyword *CONTROL_IMPLICIT_GENERAL is used to activate the implicit method. The second entry on this card is the time step. For this example the time step is 0.1 sec. Therefore, a total of 10 implicit time steps will be taken to solve this problem. The results are identical to those obtained by the explicit method as shown in Sec 3.3. For small problems, such as this 1 element example, most of the computer time is spent performing IO operations in reading the data and writing the output files. Very little CPU time is spent solving the problem. No conclusions should be made concerning the execution speed of explicit versus implicit methods on this problem. Example 4-2 Aluminum cube deformation, implicit method (file: im01.k) *KEYWORD *TITLE im01.k – implicit analysis – problem 1 $ $-------------------------- implicit solution keywords ------------------------- $ *CONTROL_IMPLICIT_GENERAL This keyword turns on the implicit method 1 .1 $ $--------------- define solution control and output parameters ---------------- $ *CONTROL_TERMINATION 1. *DATABASE_BINARY_D3PLOT LS-DYNA The Next Step $ $--------------- define model geometry and material parameters ---------------- $ *PART aluminum block 1 1 1 *SECTION_SOLID 1 *MAT_ELASTIC 1 2700. 70.e+09 .3 *NODE 1 0. 0. 0. 7 7 2 1. 0. 0. 5 0 3 1. 1. 0. 3 0 4 0. 1. 0. 6 0 5 0. 0. 1. 4 0 6 1. 0. 1. 2 0 7 1. 1. 1. 0 0 8 0. 1. 1. 1 0 *ELEMENT_SOLID 1 1 1 2 3 4 5 6 7 8 $ $---------------- define boundary conditions and load curves ------------------ $ *LOAD_SEGMENT 1 1. 0. 5 6 7 8 *DEFINE_CURVE 1 0. 0. 1. 70.e+05 LS-DYNA The Next Step 4.3 Heat Transfer Analysis (problem th01.k) LS-DYNA can solve steady state and transient heat transfer problems. Steady state problems are solved in one step, while transient problems are solved using an implicit method. Our 1-element problem will now be re-defined as a transient heat transfer problem as shown below: Q = 2.43e+07 W / m3 1m Aluminum 1100-O density modulus of elasticity Poisson Ratio coefficient of expansion heat capacity thermal conductivity 2700 kg/m3 70.e+09 Pa 0.3 23.6e-06 m/m K 900 J/kg K 220 W/m K We will solve for the temperature response of the cube as the result of internal heat generation, Q. All the surfaces of the cube are perfectly insulated. Therefore, all the heat generation goes into increasing the internal energy of the cube. The temperature response of the cube calculated by LS- DYNA is shown in the figure below. The analytical solution is shown in the box. T = Qt ρVcp T = ) t( ) ( 2.43e + 07 (2700.)(1)(900.) T = 10t The keyword input for this problem is shown below. Important things to note are: • The default initial condition is T=0 for all nodes. • The default thermal boundary condition is adiabatic (i.e. perfectly insulted). Therefore, no thermal boundary conditions need be specified for this problem. • The *CONTROL_SOLUTION keyword is used to specify this problem as thermal only. • The entry on the *PART keyword points to the definition of thermal property data LS-DYNA The Next Step Example 4-3 Aluminum cube transient heat transfer analysis (file: th01.k) set printing interval set thermal time step size specify as transient solution specify heat transfer solution *KEYWORD *TITLE th01.k – heat transfer – problem 1 $ $------------------------ thermal solution keywords ---------------------------- $ *CONTROL_SOLUTION 1 *CONTROL_THERMAL_SOLVER 1 *CONTROL_THERMAL_TIMESTEP 0 1. .1 *DATABASE_TPRINT .1 $ $--------------- define solution control and output parameters ---------------- $ *CONTROL_TERMINATION 1. *DATABASE_BINARY_D3PLOT .1 $ $--------------- define model geometry and material parameters ---------------- $ *PART aluminum block 1 1 1 *SECTION_SOLID 1 *MAT_THERMAL_ISOTROPIC 1 2700. 0 2.43e+07 904. 222. *NODE 1 0. 0. 0. 7 7 2 1. 0. 0. 5 0 3 1. 1. 0. 3 0 4 0. 1. 0. 6 0 5 0. 0. 1. 4 0 6 1. 0. 1. 2 0 7 1. 1. 1. 0 0 8 0. 1. 1. 1 0 *ELEMENT_SOLID 1 1 1 2 3 4 5 6 7 8 *END LS-DYNA The Next Step 4.4 Coupled thermal-stress analysis (problem cp01.k) In this problem, the cube is allowed to expand due to the temperature increase from internal heat generation. Keywords from the mechanical problem defined in section 4.1 and the thermal problem defined in section 4.3 are combined to define this thermal-stress problem. The keyword *MAT_ELASTIC_PLASTIC_THERMAL is used to define a material with a thermal coefficient of expansion. For this problem, α =23.6-06 m/m C. The aluminum blocks starts out at 0C (the default initial condition) and heats up 10C over the 1 second time interval . The x displacement of node 7 versus temperature increase as calculated by LS-DYNA is shown in the figure below. The curve is not smooth due to numerical noise in the solution because we are only using 1 element. The analytical solution is shown in the box. ∆x = α∆T = 23.6e − 06 ( ) ) 10( = 23.6e − 05 The keyword input for this problem is shown below. Important things to note are: • *CONTROL_SOLUTION is set to 2. This defines the problem as a coupled thermal stress analysis. • Defining both mechanical and thermal properties. • Using a mechanical constitutive model (*MAT_ELASTIC_PLASTIC_THERMAL) that allows entry of a thermal coefficient of expansion and mechanical properties that are a function of temperature. • The mechanical and thermal time steps are independent. For this problem, we are using the default explicit mechanical time step calculated by the code and have specified a thermal time LS-DYNA The Next Step Example 4-4 Aluminum cube coupled thermal-stress solution (file: cp01.k) specify thermal-stress solution *KEYWORD *TITLE cp01.k - coupled thermal stress analysis - problem 1 $ $--------------- define solution control and output parameters ---------------- $ *CONTROL_SOLUTION 2 *CONTROL_TERMINATION 1. *DATABASE_BINARY_D3PLOT .1 $ $------------------------ thermal solution keywords ---------------------------- $ *CONTROL_THERMAL_SOLVER 1 *CONTROL_THERMAL_TIMESTEP 0 1. .1 *DATABASE_TPRINT .1 $ $--------------- define model geometry and material parameters ---------------- $ *PART aluminum block 1 1 1 1 *SECTION_SOLID 1 *MAT_ELASTIC_PLASTIC_THERMAL 1 2700. 0. 100. 70.e+09 70.e+09 .3 .3 23.6e-06 23.6e-06 specify mechanical material specify thermal material *MAT_THERMAL_ISOTROPIC 1 2700. 0 2.44e+07 904. 222. *NODE 1 0. 0. 0. 7 7 2 1. 0. 0. 5 0 3 1. 1. 0. 3 0 4 0. 1. 0. 6 0 5 0. 0. 1. 4 0 6 1. 0. 1. 2 0 7 1. 1. 1. 0 0 8 0. 1. 1. 1 0 *ELEMENT_SOLID 1 1 1 2 3 4 5 6 7 8